Chapter : Introduction to ANSYS Fluent

ANSYS Fluent is a state-of-the-art computer program for modeling fluid flow, heat transfer, and chem-

ical reactions in complex geometries.

ANSYS Fluent is written in the C computer language and makes full use of the flexibility and power

offered by the language. Consequently, true dynamic memory allocation, efficient data structures, and

flexible solver control are all possible. In addition, ANSYS Fluent uses a client/server architecture, which

enables it to run as separate simultaneous processes on client desktop workstations and powerful

compute servers. This architecture allows for efficient execution, interactive control, and complete

flexibility between different types of machines or operating systems.

ANSYS Fluent provides complete mesh flexibility, including the ability to solve your flow problems using

unstructured meshes that can be generated about complex geometries with relative ease. Supported

mesh types include 2D triangular/quadrilateral, 3D tetrahedral/hexahedral/pyramid/wedge/polyhedral,

and mixed (hybrid) meshes. ANSYS Fluent also enables you to refine or coarsen your mesh based on

the flow solution.

You can read your mesh into ANSYS Fluent, or, for 3D geometries, create your mesh using the meshing

mode of Fluent (see the Fluent User’s Guide (p. ) for further details). All remaining operations are

performed within the solution mode of Fluent, including setting boundary conditions, defining fluid

properties, executing the solution, refining the mesh, and postprocessing and viewing the results.

The ANSYS Fluent serial solver manages file input and output, data storage, and flow field calculations

using a single solver process on a single computer. ANSYS Fluent also uses a utility called cortex that

manages ANSYS Fluent’s user interface and basic graphical functions. ANSYS Fluent’s parallel solver

enables you to compute a solution using multiple processes that may be executing on the same com-

puter, or on different computers in a network.

The ANSYS Fluent solver manages file input and output, data storage, and flow field calculations. Pro-

cessing involves an interaction between ANSYS Fluent, a host process, and one or more compute-node

processes. ANSYS Fluent interacts with the host process and the compute node(s) using a utility called

cortex, which manages ANSYS Fluent’s user interface and basic graphical functions.

Figure . : ANSYS Fluent Architecture

ANSYS Fluent’s serial solver uses a single compute node, whereas the parallel solver computes a solution

using multiple compute nodes that may be executing on the same computer, or on different computers

in a network.

For more information about ANSYS Fluent’s parallel processing capabilities, message passing interfaces

(MPI), and so on, refer to Parallel Processing (p. ) in the User's Guide (p. ).

All functions required to compute a solution and display the results are accessible in ANSYS Fluent

through an interactive interface.

For more information, see the following sections:

..The ANSYS Product Improvement Program

.. Program Capabilities

.. Known Limitations in ANSYS Fluent  R3

Introduction to ANSYS Fluent

This product is covered by the ANSYS Product Improvement Program, which enables ANSYS, Inc., to

collect and analyze anonymous usage data reported by our software without affecting your work or

product performance. Analyzing product usage data helps us to understand customer usage trends

and patterns, interests, and quality or performance issues. The data enable us to develop or enhance

product features that better address your needs.

How to Participate

The program is voluntary. To participate, select Yes when the Product Improvement Program dialog

appears. Only then will collection of data for this product begin.

How the Program Works

After you agree to participate, the product collects anonymous usage data during each session. When

you end the session, the collected data is sent to a secure server accessible only to authorized ANSYS

employees. After ANSYS receives the data, various statistical measures such as distributions, counts,

means, medians, modes, etc., are used to understand and analyze the data.

Data We Collect

The data we collect under the ANSYS Product Improvement Program are limited. The types and amounts

of collected data vary from product to product. Typically, the data fall into the categories listed here:

Hardware: Information about the hardware on which the product is running, such as the:

brand and type of CPU

number of processors available

amount of memory available

brand and type of graphics card

System: Configuration information about the system the product is running on, such as the:

operating system and version

country code

time zone

language used

values of environment variables used by the product

time zone

Session: Characteristics of the session, such as the:

interactive or batch setting

time duration

total CPU time used

The ANSYS Product Improvement Program

product license and license settings being used

product version and build identifiers

command line options used

number of processors used

amount of memory used

errors and warnings issued

Session Actions: Counts of certain user actions during a session, such as the number of:

project saves

restarts

meshing, solving, postprocessing, etc., actions

times the Help system is used

times wizards are used

toolbar selections

Model: Statistics of the model used in the simulation, such as the:

number and types of entities used, such as nodes, elements, cells, surfaces, primitives, etc.

number of material types, loading types, boundary conditions, species, etc.

number and types of coordinate systems used

system of units used

dimensionality (-D, -D, -D)

Analysis: Characteristics of the analysis, such as the:

physics types used

linear and nonlinear behaviors

time and frequency domains (static, steady-state, transient, modal, harmonic, etc.)

analysis options used

Solution: Characteristics of the solution performed, including:

the choice of solvers and solver options

the solution controls used, such as convergence criteria, precision settings, and tuning options

solver statistics such as the number of equations, number of load steps, number of design points, etc.

Specialty: Special options or features used, such as:

user-provided plug-ins and routines

coupling of analyses with other ANSYS products

Data We Do Not Collect

The Product Improvement Program does not collect any information that can identify you personally,

your company, or your intellectual property. This includes, but is not limited to:

names, addresses, or usernames

file names, part names, or other user-supplied labels

geometry- or design-specific inputs, such as coordinate values or locations, thicknesses, or other dimen-

sional values

actual values of material properties, loadings, or any other real-valued user-supplied data

In addition to collecting only anonymous data, we make no record of where we collect data from. We

therefore cannot associate collected data with any specific customer, company, or location.

Opting Out of the Program

You may stop your participation in the program any time you wish. To do so, select ANSYS Product

Improvement Program from the Help menu. A dialog appears and asks if you want to continue parti-

cipating in the program. Select No and then click OK. Data will no longer be collected or sent.

The ANSYS, Inc., Privacy Policy

All ANSYS products are covered by the ANSYS, Inc., Privacy Policy.

Frequently Asked Questions

. Am I required to participate in this program?

No, your participation is voluntary. We encourage you to participate, however, as it helps us create

products that will better meet your future needs.

. Am I automatically enrolled in this program?

No. You are not enrolled unless you explicitly agree to participate.

. Does participating in this program put my intellectual property at risk of being collected or discovered by ANSYS?

No. We do not collect any project-specific, company-specific, or model-specific information.

. Can I stop participating even after I agree to participate?

Yes, you can stop participating at any time. To do so, select ANSYS Product Improvement Program

from the Help menu. A dialog appears and asks if you want to continue participating in the program.

Select No and then click OK. Data will no longer be collected or sent.

. Will participation in the program slow the performance of the product?

No, the data collection does not affect the product performance in any significant way. The amount

of data collected is very small.

. How frequently is data collected and sent to ANSYS servers?

The data is collected during each use session of the product. The collected data is sent to a secure

server once per session, when you exit the product.

. Is this program available in all ANSYS products?

Not at this time, although we are adding it to more of our products at each release. The program

is available in a product only if this ANSYS Product Improvement Program description appears in the

product documentation, as it does here for this product.

. If I enroll in the program for this product, am I automatically enrolled in the program for the other ANSYS products

I use on the same machine?

Yes. Your enrollment choice applies to all ANSYS products you use on the same machine. Similarly,

if you end your enrollment in the program for one product, you end your enrollment for all ANSYS

products on that machine.

. How is enrollment in the Product Improvement Program determined if I use ANSYS products in a cluster?

In a cluster configuration, the Product Improvement Program enrollment is determined by the host

machine setting.

. Can I easily opt out of the Product Improvement Program for all clients in my network installation?

Yes. Perform the following steps on the file server:

a.

Navigate to the installation directory: [Drive:]\v195\commonfiles\globalsettings

b. Open the file ANSYSProductImprovementProgram.txt.

c.

Change the value from "on" to "off" and save the file.

When in meshing mode, ANSYS Fluent functions as a robust unstructured-volume-mesh generator (see

Meshing Mode Capabilities (p. ) in the Fluent User’s Guide (p. ) for further details). When in solution

mode, Fluent allows you to simulate the following:

2D planar, 2D axisymmetric, 2D axisymmetric with swirl (rotationally symmetric), and 3D flows

Flows on quadrilateral, triangular, hexahedral (brick), tetrahedral, wedge, pyramid, polyhedral, and mixed

element meshes

Steady-state or transient flows

Incompressible or compressible flows, including all speed regimes (low subsonic, transonic, supersonic, and

hypersonic flows)

Inviscid, laminar, and turbulent flows

Newtonian or non-Newtonian flows

Ideal or real gases

Heat transfer, including forced, natural, and mixed convection, conjugate (solid/fluid) heat transfer, and ra-

diation

Chemical species mixing and reaction, including homogeneous and heterogeneous combustion models

and surface deposition/reaction models

diation

Free surface and multiphase models for gas-liquid, gas-solid, and liquid-solid flows

Lagrangian trajectory calculations for dispersed phase (particles/droplets/bubbles), including coupling with

continuous phase and spray modeling

Cavitation model simulations

Melting/solidification applications using the phase change model

Porous media with non-isotropic permeability, inertial resistance, solid heat conduction, and porous-face

pressure jump conditions

Lumped parameter models for fans, pumps, radiators, and heat exchangers

Acoustic models for predicting flow-induced noise

Inertial (stationary) or non-inertial (rotating or accelerating) reference frames

Multiple moving frames using multiple reference frame (MRF) and sliding mesh options

Mixing-plane model simulations of rotor-stator interactions, torque converters, and similar turbomachinery

applications with options for mass conservation and swirl conservation

Dynamic mesh model simulations for domains with moving and deforming meshes

Volumetric sources of mass, momentum, heat, and chemical species

Simulations that use a material property database

Simulations in which the design is revised or optimized, using the adjoint solver or the mesh

morpher/optimizer

Simulations customized by user-defined functions

Dynamic (two-way) coupling with GT-POWER and WAVE

Simulations that use the following add-on modules:

– Battery module

– Continuous fiber module

– Macroscopic particle model (MPM) module

– Fuel cell modules

– Magnetohydrodynamics (MHD) module

– Population balance module

Program Capabilities

Fluent as a Server (documented separately)

ANSYS Fluent is ideally suited for incompressible and compressible fluid-flow simulations in complex

geometries. ANSYS Fluent’s parallel solver enables you to compute solutions for cases with very large

meshes on multiple processors, either on the same computer or on different computers in a network.

ANSYS, Inc. also offers other solvers that address different flow regimes and incorporate alternative

physical models. Additional CFD programs from ANSYS, Inc. include CFX, ANSYS Icepak, and ANSYS

Polyflow.

This section lists limitations that are known to exist in ANSYS Fluent. Where possible, suggested work-

arounds are provided.

File import/export (for a list of supported files, refer to the table in this section, under Third-party software)

– (Windows only) ANSYS Fluent cannot import CGNS files greater than  GB in size. ()

– Due to a 3rd party issue, Mechanical APDL results files using sparsification file compression (default

at ANSYS Release  R3) cannot be read into Fluent and may cause the session to close unexpec-

tedly. As a workaround, you can un-compress these files using the *XPL command in Mechanical

APDL (refer to the UNCOMP value of the COPY action described in X Commands in the Command

Reference)

– If you change the File Storage Options settings in the Autosave dialog box, the solution history will be

lost.

– When exporting EnSight Case Gold files for transient simulations, the solver cannot be switched between

lost.

serial and parallel, and the number of compute nodes cannot be changed for a given parallel run. Otherwise,

the exported EnSight Case Gold files for each time step will not be compatible.

– EnSight export with topology changes is not supported.

– To properly view Fieldview Unstructured (.fvuns) results from a serial or parallel ANSYS Fluent simulation:

→ Mesh files must be exported using the fieldview-unstruct-grid text command.

→ Mesh and data files should all be exported from parallel ANSYS Fluent sessions with the same number

of nodes.

– Tecplot file import does not support the Tecplot360 file format.

– The maximum number of profiles that can be read into a single Fluent session is .

– The PARALLEL INDEPENDENT mode for Hierarchical Data Format file I/O is known to exhibit slow write

performance. On parallel file systems, consider using the PARALLEL COLLECTIVE mode when writing HDF

files. On other network file systems, consider using the HOST or NODE0 mode.

– If you are accessing a file using a Universal Naming Convention (UNC) path, you must ensure that you

have permission to access to all of the folders in the path or you will not be able to open the file.

– (Windows only) The file filter available in the Select File dialog box may not work as expected, requiring

you to manually select the desired file(s) without filtering aid. ()

– Files written by ANSYS products do not support synchronization with Microsoft's OneDrive file hosting

service. ( / )

– When you have read a mesh or case file in Fluent, you cannot then append a case file that uses the Hier-

archical Data Format (HDF)—that is, a .cas.h5 file. Workaround: If one of the case files does not use

HDF, then read the HDF case file first and append the other file. ()

Mesh

– Boundary zone extrusion is not possible from faces that have hanging nodes.

– For simulations that involve the Fluent, Mechanical, and Meshing applications, meshing problems can

arise in instances where there are multiple regions and contacts between them. In Fluent, a zone can only

exist in a single contact region.The Mechanical and Meshing applications both use a different approach

concerning contact regions when compared to Fluent.

– ANSYS Fluent does not support FSI data mapping of edges and, therefore, it is not supported in 2D.

– At non-conformal interfaces, the Matching option is no longer allowed with the Mapped option.When

opening a case set up in a previous release with both options enabled, you will be prompted to recreate

the interface without the Matching option.

– If your mesh topology has a step-wise prism mesh near the walls, do not use node-based gradients with

MUSCL.

– For shell conduction cases in which you have performed adaption using the polyhedral unstructured

mesh adaption (PUMA) method, ANSYS Fluent may terminate abnormally if you attempt to improve

mesh quality in a parallel session with multiple compute nodes. Workaround: After adapting with

the PUMA method, you must save the case file and read it back into Fluent before improving mesh

quality.

Models

– Fluent allows you to select via System Coupling as a thermal boundary condition option on the

quality.

Models

child zone of a sliding interface. This is not supported, and the .scp file correctly suppresses that

region from coupling.

– ANSYS Fluent supports the Chemkin II format for Oppdif flamelet import only.

– The surface-to-surface (S2S) radiation model does not work with moving/deforming meshes.

– The DPM work pile algorithm is not compatible with the wall film boundary condition.

– For transient Lagrangian multiphase analysis with DPM unsteady particle tracking, atomizer or cone injec-

tions will release particles from the same position rather than from random positions if Particle Time

Step Size is smaller than Time Step Size.To use random starting points for the particles, enter the following

Scheme commands in the ANSYS Fluentconsole:

(rpsetvar 'dpm/random/seed-timestep-corrected? #t)

(dpm-parameters-changed)

Note that this change will also affect particle trajectories if stochastic tracking, particle breakup, or

other mechanisms that involve random numbers are used. ()

Known Limitations in ANSYS Fluent  R3

– The shell conduction model is not applicable on moving walls.

– The heat exchanger model is not compatible with mesh adaption.

– The Fluent/ANSYS Reaction Design KINetics coupling is not available on the win64 platform.

– DO-Energy coupling is recommended for large optical thickness cases (> ) only.

– FMG initialization is not available with the shell conduction model.

– FMG initialization is not compatible with the unsteady solver.

– The MHD module is not compatible with Eulerian multiphase models.

– Bounded 2nd order discretization in time is not compatible with moving and deforming meshes.

– When simulating porous media, the value of the Porosity (defined in the Fluid dialog box) cannot be

or  (that is, it must be in between these values) if the non-equilibrium thermal model is enabled.

– When simulating porous media, the non-equilibrium thermal model is not supported with radiation and/or

multiphase models.

– For porous media simulations, the relative velocity resistance formulation is not supported with axisym-

metric-swirl when there are non-zero swirl resistances.

– The junction of a wall with shell conduction enabled and a non-conformal coupled wall is not supported.

Such a junction will not be thermally connected, that is, there will be no heat transfer between the shell

and the mesh interface wall.

– After you enable the Eulerian Wall Film model, Fluent will not allow you to save the mesh modifications,

such as separating cells, extruding face zones, and changing the cell zones type. If you want to modify

the mesh in Fluent, be sure to complete all mesh operations prior to enabling the Eulerian Wall Film

model.

– The Transition SST model (also known as the γ-Reθ model) is not Galilean invariant and should therefore

not be applied to surfaces that move relative to the coordinate system for which the velocity field is

computed; for such cases, the Intermittency Transition model (also known as the γ model) should be used

instead.

– In simulations that use the discrete phase model, particle mass may be lost when simulation of transient

particles released with constant parcel size is combined with auto-save of case files.

– User-defined wall functions are not compatible with the Eulerian multiphase formulation and cannot be

used.

– The view factor files generated as part of a surface-to-surface radiation model calculation for version .

or . of Fluent may not be compatible with newer versions if the Matching option was enabled for a

mapped interface. For any case file with such a setup, you must recompute the view factors in the newer

version to ensure correct results.

Parallel processing

– The discrete transfer radiation model (DTRM) is unavailable in the parallel solver.

– Mellanox OFED version ..–.. is known to cause random crashes or startup issues in Fluent when

using core counts greater than approximately .The last known stable Mellanox version is ...You

may use either of the following as a workaround:

→ Revert to OFED ...

→ Set the value of log_num_mtt to  in the mlx4_core driver on all machines.

– IBM MPI does not support running in parallel in an overload condition (using more cores than are physically

available on a machine). For performance reasons, running in an overload condition is generally not re-

commended. However, if it is required to run overloaded, then you can use Intel MPI (-mpi=intel) or

Open MPI (-mpi=openmpi).

– The version of IBM MPI that is distributed with Fluent is now limited to a maximum of  processes for

a single simulation. For higher core counts, an additional license is required. Refer to IBM Platform MPI

with High (>) Process Count in the ANSYS, Inc. Installation Guides for more information.

– Note that on systems using large pages for memory allocation (such as Cray), the virtual memory usage

reported by Fluent may be much higher than actual memory used. In this case resident memory (also

reported by Fluent) is a more reliable guide.

– Degenerate contact points are known to cause topological mesh connectivity issues in parallel. Degenerate

contact points are nodes that are shared by  or more cell zones that do not share faces. Fluent can detect

degenerate contact points in serial via a mesh check with the mesh check verbosity set greater than . If

a case has generate contact points then you must use the following command before reading the case

for proper parallel handling of such contact points.

(rpsetvar 'parallel/add-dgcp-to-int-or-corner?)

– The Eulerian Wall-film model is not compatible with the DPM Domain option of the hybrid parallel DPM

tracking. For such model combination, the Use DPM Domain option must be disabled in the Parallel tab

of the Discrete Phase Model dialog box.

– The Fluent process binding (affinity) setting is not supported for Windows machines with more than

cores that are using the IBM MPI communication library, which may increase processing time. As a work-

around, you can use Intel MPI or disable hyper-threading (if the machine has Intel processors) to lower

the core count to be equal to or below .

– Starting in version ., ANSYS Fluent will require approximately  MB more memory per node process

compared to version .–..

– If you have OpenSSH inside C:\windows\system32 and want to run a mixed Windows-Linux simu-

lation, Fluent may not be able to locate and execute the ssh command, and the following warning

will be printed:

'ssh' is not recognized as an internal or external command, operable

program or batch file.

You must specify the path of the actual ssh to be used: launching from the command line, use the

rsh option (for example, -rsh=c:\cygwin64\bin\ssh.exe); using Fluent Launcher, select

Other from the Remote Spawn Control list in the Remote tab and enter the path in the text box

(for example, c:\cygwin64\bin\ssh.exe).

In addition, you should add the location of ssh executable to the beginning of the PATH environ-

ment variable. (/)

– The Intel MPI version upgrade in Fluent release  R1 breaks compatibility with older releases on Win-

dows. Workaround: To switch between running older releases and the latest release on a cluster, you

must make sure that the appropriate services have been configured to run by the administrator as follows:

→ To switch from old to new (for example, . to  R1), run the following command on all nodes

from the command prompt with administrator privileges:

“C:\Program Files (x86)\IntelSWTools\compilers_and_libraries_2018..\windows\mpi\intel64\bin\

hydra_service.exe” -install

→ To switch from new to old (for example,  R1 to . ), run the following command on all nodes

“C:\Program Files (x86)\IntelSWTools\compilers_and_libraries_2017..\windows\mpi\intel64\bin\

After installing both versions of Intel MPI, the I_MPI_ROOT environment variable should be deleted

from all nodes.

()

()

Platform support and drivers

– On Windows Server OS, ANSYS Fluent supports only MS MPI for parallel runs. Installing any other unsup-

ported MPI libraries (IBM MPI or Intel MPI) will result in conflicts.

– On Windows  and later, installing ANSYS Fluent on any drive other than C: may result in issues arising

from spaces in the pathname not getting converted to short file names.This is the result of a change in

the default value for NtfsDisable8dot3NameCreation starting with Windows . If you need to install

ANSYS Fluent on any drive other than C: you must run the following command prior to installing ANSYS

Fluent:

fsutil 8dot3name set <driveletter>

where <driveletter> is the target drive letter including the colon (for example, D:).

– The minimum OS requirements for Linux are SLES  SP2 or RHEL .

– The pathname length to the cpropep.so library (including the lib name) is limited to  characters. (Linux

Opteron cluster using Infiniband interconnect only.)

– On Linux platforms, including a space character in the current working directory path is not supported.

– If you are installing ANSYS Fluent  R3 on a Windows machine that already has one or more previous

versions of ANSYS Fluent, then after installing IBM MPI and Intel MPI libraries from the prerequisites, make

sure to delete the environment variables MPI_ROOT (for IBM MPI) and I_MPI_ROOT (for Intel MPI). Otherwise

there will be a conflict while running previous ANSYS Fluent versions in parallel mode.

– Remote Solver Facility (RSF) is no longer supported in ANSYS Fluent.

– Itanium platform (lnia64) is no longer supported.

– ANSYS Fluent uses several TCP/IP ports for communications and error handling. Port conflicts with other

programs trying to use the same ports are handled by ANSYS Fluent and generate warnings similar to

the following:

: mpt_accept: warning: incorrect exercise message "GET /" from ... on port

Long running large sessions are more prone to generating such warnings, but these are generally

safe for you to ignore.

– When using the default MPI (ibmmpi) on some newer hardware the following message may appear when

exiting the Fluent session.

hwloc has encountered what looks like an error from the operating system.

object (Socket cpuset 0xff00ffff) intersection without inclusion!

Error occurred in topology.c line

Please report this error message to the hwloc user's mailing list,

along with any relevant topology information from your platform.

This message is from the hardware locality library used by IBM MPI. You can set the following en-

vironment variable to hide this message, or switch to Intel MPI.

HWLOC_HIDE_ERRORS=

– If you lock the computer screen before the Fluent graphics are initialized, the Fluent session will not launch

if you are using the OpenGL graphics driver.To avoid this issue with the OpenGL driver, you can use the

alternative drivers x11 or null for Linux/unix and msw or null for Windows.You can specify an alternate

graphics driver either by defining it in the HOOPS_PICTURE environment variable or using the -driver

Fluent command line option.

– Fluent may terminate abnormally during launch when running on Community Enterprise OS (CentOS)

. or Red Hat Enterprise Linux (RHEL) . when DISPLAY is set to a Virtual Network Computing (VNC)

session.To attempt to resolve this, verify that you are using a supported graphics card and update the

graphics card drivers (directly from the graphics card vendor website). If the issue persists, you can do

one of the following: set the DISPLAY to a local machine; set the LD_PRELOAD environment variable to

/usr/lib64/libstdc++.so. ; or use the alternative drivers x11 or null (either by defining it in

the HOOPS_PICTURE environment variable or using the -driver Fluent command line option).

– When launching Fluent (in meshing mode or solution mode) on Windows with the default IBM MPI, if the

installation path is very long, then you may receive the following error message and be forced to use the

Task Manager to end the Fluent application:

mpirun.exe has stopped working

As a workaround, you can avoid this issue by using the Intel MPI (note that in Fluent Launcher,

you can only revise the MPI as part of parallel settings, so for a serial case you need to select par-

allel with a single processor); or, you can try minimizing the number of characters in the Fluent

installation path. ()

Remote display

– Connecting or disconnecting a VPN network while running a Fluent simulation will result in a failure because

of changes to the network interface.

– If you experience an abnormal termination when running Fluent via a remote display, check you graphics

card to ensure that you have a modern professional graphics card that is up-to-date (that is, the latest

updated driver for that card, which is available on the company's website). If your system does not meet

the graphics card requirements, launch Fluent using a completely software-based driver, such as MSW

(Windows) or X11 (Linux).

– (Exceed onDemand and VNC Viewer) The Num Lock number keys and arrows may not function in the

graphical user interface or console. As a workaround, you can define the XKB_DEFAULT_RULES envir-

onment variable set equal to base, which resolves the arrow keys' functionality. Number entries must

still be completed using the number keys at the top of the standard keyboard. ()

– (Linux only) When running ANSYS Fluent using the Virtual Network Computing (VNC), Nice DCV, or Exceed

on Demand (EoD) applications, you may experience unexpected error messages due to a 3rd party issue.

To resolve these errors, install the following packages: ()

→ xcb-util-wm-..-.el6.x86_64

→ xcb-util-keysyms-..-.el6.x86_64

→ xcb-util-..-..el6.x86_64

→ compat-xcb-util-..-..el6.x86_64

→ xcb-util-image-..-.el6.x86_64

– (Linux only) On some clusters without accelerated graphics, Fluent may not accept keyboard inputs. If

you encounter this behavior, set the QT_XKB_CONFIG_ROOT environment variable equal to

/usr/share/X11/xkb.

Cell Zones and Boundary Conditions

– A reference frame is always displayed at its initial state (position and orientation) when displayed from

the Reference Frame dialog box.While running a transient simulation for multiple time steps, a reference

frame is displayed at its current state. After the calculation is completed, if you open the Reference Frame

dialog box and display it, the reference frame triad will move back to its initial state. ()

– Clicking OK within the Reference Frame dialog box will reset a reference frame to its initial state. If you

do not intend to make changes to a reference frame, leave the dialog box by clicking Cancel. ()

Reference Frames

– Fluid zones designated as 3D fan zones cannot have non-conformal interfaces.

Solver

– The absolute and relative velocity formulations may yield different results in cases where a strong reversal

of flow exists at a pressure outlet boundary.

– The non-iterative time advancement (NITA) solver is applicable with only a limited set of models. See the

ANSYS Fluent User's Guide for more details.

– NITA (using fractional time step method) is not compatible with porous media.

– The following models are not available for the density-based solvers:

→ Volume-of-fluid (VOF) model

→ Multiphase mixture model

→ Eulerian multiphase model

→ Non-premixed combustion model

→ Premixed combustion model

→ Partially premixed combustion model

→ Composition PDF transport model

→ Soot model

→ Rosseland radiation model

→ Melting/solidification model

→ Enhanced Coherent Flamelet model

→ Inert model: transport of inert species (EGR in IC engines)

→ Dense discrete phase model

→ Shell conduction model

→ Floating operating pressure

→ Spark ignition and auto-ignition models

→ Physical velocity formulation for porous media

→ Selective multigrid (SAMG)

– The pressure-based coupled solver is not available with the following features:

→ Fixed velocity

– On some Linux platforms, pressing Ctrl+C will not interrupt the solution. A suggested workaround is to

use the checkpoint mechanism in Fluent to save files and/or exit Fluent. (Checkpointing an ANSYS Flu-

ent Simulation in the Fluent User's Guide (p. ))

– In certain cases with tetrahedral or hybrid meshes, the use of the Least-Squares Cell Based gradient

method in combination with the cell-to-cell limiter may cause divergence. If this is observed, it is recom-

mended that you either change the gradient method to Green-Gauss Node Based or change the limiter

type to the cell-to-face limiter.

– Beginning in version ., the warped-face gradient correction (WFGC) is not supported with shell con-

duction if the ability to define multi-layer shells has been disabled through the define/models/shell-

conduction/multi-layer-shell text command.

– For transient and time-dependent cases, the solution advances to the next time step based on various

inputs including time step size and convergence criteria, but it is not directly dependent on the flow time

interval specified when 'flow-time' is selected for monitoring (report definitions, autosaving, transient

export and so on). For these flow time dependent operations, the action will occur when the flow time

meets or exceeds the specified flow time interval.

– Note the following issues affecting residuals:

→ Restarting cases that have the High Order Term Relaxation option enabled may produce a small re-

sidual jump after the restart. ()

→ Restarting cases that have turbulent flow with a wall-function-based boundary treatment and a No

Slip shear condition at the wall may produce a slightly different residual history compared to a continu-

ous run. ()

These issues can occasionally impact the residual history of long transient simulations (such as

those that use the LES, SRS, or SBES model) when the solutions for each time step are not deeply

converged.

– For case files created in Release . or earlier and are steady, single phase, and use the pressure-based

solver, the Density explicit relaxation factor in the Solution Controls task page is set to  in the following

circumstances, even though it should be set to . (in order to match how a case file created in Release

R1 would behave):

→ if the physics includes reacting flow and/or species transport together with the pseudo transient solution

method, and you click the Default button in the Solution Controls task page

→ if you newly enable one or both of the following so that both are enabled:

a reacting flow model and/or the species transport model

the pseudo transient solution method

Work-around: Manually enter . for Density in the Solution Controls task page. ()

– The following text command works appropriately for setting limits to default values, but fails to take action

on solution controls and AMG controls:

> solve/set/set-controls-to-default

Set solution controls to default? [no] yes

Set AMG Controls to default? [no] yes

Set limits to default values? [no] yes

Work-around: Click the Default button in the Solution Controls task page and the Multigrid tab

of the Advanced Solution Controls dialog box, respectively. As noted previously, for older steady-

state, single-phase cases that use the pressure-based solver and involve reacting flow and/or species

transport with the pseudo transient solution method, you must also manually set the Density ex-

plicit relaxation factor to . in the Solution Controls task page. ()

User-Defined

– Any scripts or journals that attempt to add menu items to Fluent pull-down menus (which have been re-

placed with the Fluent ribbon) will no longer work.You must create separate user-defined menus to

house all user-defined menu items. For additional information about user-defined menus, see Adding

Menus to the Right of the Ribbon in the Fluent Customization Manual.

User-defined functions (UDFs)

– Interpreted UDFs cannot be used with an Infiniband interconnect or, when running in parallel, on the

Cray platform.The compiled UDF approach must be used instead.

– The Visual Studio Express  for Windows installer on Windows  installs libraries in non-standard

locations, resulting in UDF compilation failures on this platform. It is recommended that you instead use

the Visual Studio Express  for Desktop installer, or manually set the library path based on your

local installation (for example, LIB="C:\Program Files (x86)\Microsoft Visual Studio

.\VC\lib\onecore\amd64";%LIB%).

Graphics, Reporting, and Postprocessing

– Monitors may continue to print/plot values, even if the zones on which they are defined are deactivated.

– If you are autosaving multiple scenes on a Windows machine, the Headlight lighting effect may incon-

sistently change its state (on/off).This can be avoided by rendering each scene in a separate graphics

window.

– Mean and root-mean-squared-error (RMSE) quantities of custom field functions are only available for

mixtures. In previous releases it was possible to specify these quantities for phases, which was an incorrect

behavior.This behavior is no longer allowed in R16. or later releases. If you are running a pre-R16. case

set to output such quantities in R2019 R3, you may get a segmentation error.To avoid the error, redefine

the previously defined monitors reporting mean or RMSE quantities of phases.

– The mouse-annotate feature is no longer available. Annotations can still be created using the Annotate

dialog box (see Annotate Dialog Box in the Fluent User's Guide (p. ) for additional information).

– Beginning in version ., if a flux report for the heat transfer rate is generated on the wall of a moving

solid, the reported values will include the convective heat flux due to the motion of the solid. Depending

on the mesh and quality of the geometry representation, this may present flux values that are different

than the flux specified in the boundary condition definition (for example, a non-zero flux may be reported

for an adiabatic wall).

– Beginning in version ., if you import a legacy case containing multiple monitors plotting in the same

window, you must review the setup to ensure each report plot is assigned to a different window before

running the calculation. If the plot windows are not reassigned, then plots assigned to the same window

will be lost.

– It is possible to use text commands to create contour, vector, mesh, pathline, particle track, XY plot, and

scene graphics objects with spaces in the name (for example, through the display/objects/create

text command); however, objects with such names cannot be displayed using the display/ob-

jects/display text command, and attempting to do so will only result in the printing of an error. As

a workaround, you can create graphics objects without spaces in the name or use the graphical user in-

terface to display graphics objects with spaces in the name.

– In rare cases, the Curve Length X Axis Function for XY plots may not plot correctly, even if the curvilinear

surface is piecewise linear and appears to be a single closed curve. A workaround is to use the Direction

Vector X Axis Function.

– Transient statistics (Mean and RMS) reported for Fluent quantities that are nonlinear functions of the un-

derlying solution variables represent evaluations of those quantities using the Mean or RMS values of the

underlying solution variables. For instance, Mean Velocity Magnitude is computed as the magnitude of

a vector constructed from the mean velocity components, and Mean Pressure Coefficient is computed

as the pressure coefficient computed using the mean pressure.To construct the true Mean and/or RMS

values of such quantities, you can define a custom field function and collect transient statistics of the

custom field function. For example, define a custom field function vmag_cff = sqrt (Vx ^  + Vy ^  +

Vz ^ ), and report Mean and RMS of vmag_cff.

– Scene animations created using Key Frames in the Animate dialog box are not compatible with graphics

displays on isosurfaces (contours, vectors, pathlines, particle tracks). Pathlines are not compatible with

scene animations, regardless of the selected surface(s).

– When meshes contain a large number of cells (for example, ~ million cells or higher), the meshing

mode of Fluent may report an incorrect number of skewed cells, based on an incorrect inverse orthoskew

(IOS) value. As a workaround, you can use the (tgapi-util-set-number-of-parallel-compute-

threads ) command. ()

– If you create an XY plot for display on a rake surface and you use the savable XY plot graphics object, ac-

cessed by clicking New... in the ribbon or outline view, then the results may not be displayed immediately.

If they do not appear, click Curves... in the XY Plot dialog box and select a Symbol from the drop-down

list in the Marker Style group box, click Apply, then redisplay the XY plot. ()

If you are viewing cell values (Node Values disabled) on an XY plot of a rake surface and the points

are being shown as a continuous line, then you can change the Pattern to "empty" in the Curves

Solution XY Plot dialog box (Line Style group box). ()

– The transform operation in the Transform Surface dialog box is not available for user-created

surfaces such as lines, points, iso-surfaces, and so on. To create a transformed line, point, iso-surface,

or other user-created surface, you must manually translate the input point(s) and create a new

line/point/iso-surface in the respective dialog box (Line/Rake, Point Surface, Iso-Surface, and so

on).

– Density contour plots that include a solid region in the display will include the solid zone(s) in any range

calculations and will show a density for the solid that does not reflect the actual case setup. Fluid zone

densities are still displayed correctly. Selecting Density... and Density All in the Contours of drop-down

lists will correctly display density values for solids and fluids. ()

– Special characters (/^*%@,<>{}()?&~!=) should not be used in object names: they can affect how an object

is rendered in the graphics display, and may make it so the object does not appear at all. ()

– For annotations, the foreground and background color options for text are not in sync with those

specified in Preferences, but are instead controlled using the display/set/colors/fore-

ground and display/set/colors/background text commands, respectively.

– For any meshing mode or solution mode session that displays graphics in the graphics window (including

when running a batch job with the -gu command line option) and/or saves picture files, the rendering

/ saving speed will be significantly slower if you do not follow all of the following best practices:

→ Run Cortex on a suitable machine with an appropriate graphics card and the latest drivers (for

details, see the ANSYS website). Note that you can assign Cortex to a particular machine using

the -gui_machine=<hostname> command line option, or by selecting Specify Machine

from the Graphics Display Machine list in the Scheduler tab of Fluent Launcher.

→ Ensure that Cortex / the host process is run on a separate machine than that used for compute node

. For example, do not include the machine assigned using the -gui_machine option as the first

machine in the hosts file / machine list (specified using the -cnf=x command line option).

→ Do not set the graphics driver to null, x11 (for Linux), or msw (for Windows).

→ When saving picture files, enable the Fast hardcopy option in the Preferences dialog box (under

Graphics).

– Right-clicking point surfaces to display them from the Outline View tree is not working due to a

3rd party issue. As a workaround, you can display point surfaces using the Mesh Display dialog

box. ()

Fluent in Workbench

– (For ROM) Clearing the Geometry or Mesh cells in a Fluent fluid flow system created in a previous

release may prevent the ROM from being created. Recreate the Fluent mesh using the latest release

to allow for ROM creation. ()

– Coupling between Fluent and HFSS or Q3D Extractor is not supported.

– For two-way coupling between Maxwell and Fluent, by default Fluent uses the following zones: when

mapping volumetric losses, the same list of zones that you selected for receiving volumetric losses in

Fluent's Maxwell Mapping Volumetric dialog box are used; and when mapping surface losses, all cell

zones are used.To change the zones that are used for feedback mapping, you can use a Scheme command,

shown in the following example.This example specifies that only cell zone ID  and  are used: (em-

set-feedback-map-cell-zone '( )). Note that you can only specify the IDs of the cell zones

as the arguments.

– In a Fluent analysis system, the Clear Generated Data option for the Solution cell will not clear the files

associated with animations.To have the Clear Generated Data option clear the animation files as well,

you must define the FLUENT_WB_REMOVE ALL_GENERATE_FILES as a system environment variable

on your local machine, prior to opening Workbench.

Fluent as a Server

– When running Fluent with the -aaS option, if you have a mesh with a very low cell count and have set

a large number of iterations to be stored using the Residual Monitors dialog box (see Storing Residual

History Points in the Fluent User's Guide (p. )), you will see a relative degradation of performance. Reducing

the number of stored iterations will reduce this degradation.

– When launching Fluent with the -gu or -g command line options and Fluent as a server enabled, Fluent

will run with the graphic user interface minimized.

Third-party software

– Fluent-Platform LSF integration is not supported on the MS Windows platform.

– Fluent-SGE integration is supported only on Linux platforms.

– Wave and GT-POWER coupling are available only with stand-alone ANSYS Fluent and not in the Workbench

environment.

– Supported versions of third-party software are listed below:

Table . : Supported Versions of Third-Party Software

Supported Version

Third-Party Software

. ODB Library: ..

Abaqus

Abaqus

.

Altair HYPERMESH

.

AVS

..

CGNS

. *

Cray MPI (MPT)

.

Data Explorer

Ensight

EnSight  (TUI only)

..

EnSight Case Gold

.

FAST

.

Fieldview

v2018 Build

GT-POWER

.-

HOOPS

... (Windows) and ... (Linux)

HP/IBM MPI

I-deas NX Series

I-deas

..**

Intel MPI

..

libpng

.

LSTC-DYNA

..

Microsoft MPI

..

MPCCI

Bulk data input file - MSC.NASTRAN

NASTRAN

OUTPUT2 data file - NX/NASTRAN

.

NIST

..***

Open MPI

.

PATRAN

PTC/Mechanica Wildfire .

PTC MECHANICA

..

Sundials

Tecplot file format, version .

TECPLOT

..

VKI

.

WAVE

..

zlib

When using MPT version . and higher (up to, but not including . ), you must set the following

environment variable: export FLUENT_USE_CRAY_MPT5=.

** By default, the Intel MPI may fail when mixing hardware for compute nodes. As a workaround,

you can use the following environment setting:

I_MPI_PLATFORM zero

*** This version of Open MPI is dependent on the following versions (or higher) of software:

→ OFED version .

→ LSF version .

→ UGE version .

→ PBS version ..

Other

– If the network connection is lost during a serial or parallel calculation, the Fluent session may terminate

abnormally.

– The IRIS Image and HPGL hard copy formats are no longer supported in ANSYS Fluent.

– When using ANSYS Fluent with the Remote Solve Manager (RSM):

→ Only one copy of a saved project that is in the pending state can reconnect successfully.

→ Maxwell coupling is not supported.

→ UDFs are supported with limitations as detailed in Submitting Fluent Jobs to Remote Solve Manager

in Workbench User's Guide.

– The turbo-averaged contour plot in turbomachinery postprocessing may give an unexpected contour

region in a selected topology.

– The Inverse Distance and Least Squares profile interpolation methods are not applicable when a profile

is attached to cell zones.

– Heat exchanger networks are not supported in HDF-formatted case and data files.

– When opening ANSYS Help from Fluent in Linux, you may receive an error message in the Linux console.

This can result when another user has created the installation and run Fluent, thus creating a registry file;

if you then run this same installation, there will be a permissions conflict. As a workaround, remove the

registry file:

path/ansys_inc/v195/Tools/mono/Linux64/etc/mono/registry

(where path is the directory in which you have placed the release directory). Then change the

permissions for the Mono platform in order to remove write access from the directory:

path/ansys_inc/v195/Tools/mono/Linux64/etc/mono

– On Windows, mesh reading into a serial ANSYS Fluent session may fail if you use more than  million

cells per core.

– For non-conformal interfaces, the use of the Matching option with the Mapped option is not recommen-

ded, especially if the extents of Interface Zone  and Interface Zone  do not coincide.

– Fluent does not support non-ASCII characters in the names of files, zones, and boundaries.

– When exiting a Fluent session on Linux that was started with the Load ACT option, Fluent may become

unresponsive. If this occurs, the Fluent process must be manually terminated. In the console, the error

message specifies that a corrupted double-linked list is responsible for the error. Because this unexpected

shutdown occurs after the project has been saved, no data is lost.

– When Fluent is run on Linux with the Load ACT option, Fluent may repeatedly issue the following warning

during solution iteration:

Unexpected error checking licensing server.

This warning is harmless and does not impact Fluent or ACT usage.

– When running a stand-alone instance of Fluent in a mixed Windows / Linux configuration or from a remote

Windows installation, ACT does not open.To correct the problem, you must set the AWP_ROOT195 en-

vironment variable to point to the ANSYS installation directory.

– ACT with ANSYS Fluent is disabled on Linux systems starting in Release ..To use ACT with ANSYS

Fluent, use Release . or later on Windows or use Release . on Linux. ()

– If you set the number of meshing processes to  (with the goal of reverting to a version of Fluent that is

similar to serial from R18. ), your request will be ignored if you have specified a nonzero value for the

number of solver processes. In such circumstances, the number of solver processes will be used for

launching both meshing and solver modes.

– If the network connection is lost during a serial or parallel calculation, the ANSYS Fluent session may ter-

minate abnormally.

the following

save for you to ignore.

Remote Visualization Client

– On some Linux machines you may see a warning message containing SO_REUSEPORT printed in the

console when starting the server.This message can be ignored—it will not have any effect on the simulation

or on the Remote Visualization Client. ()

– For a client session with multiple connected servers, only one server can receive commands through the

Send Command to Server dialog box—that server is whichever one you send a command to first using

this dialog box. As a workaround, you can use the Python console to control the other connected servers.

()

Fluent Meshing

– Limitations related to the Fluent guided meshing workflows are documented separately. See Limitations

of the Fluent Guided Workflows (p. ) for details.

– After ANSYS Fluent ., you can no longer have multiple interior zones defined in a single cell zone. If

your case file has such zones, they will not appear as available zones. Workaround: Read the mesh file

into ANSYS Fluent ., and set the type for the interior zones to be 'wall' in order to restore the missing

zones. ()

Chapter : Basic Steps for CFD Analysis using ANSYS Fluent

zones. ()

Before you begin your CFD analysis using ANSYS Fluent, careful consideration of the following issues

will contribute significantly to the success of your modeling effort. Also, when you are planning a CFD

project, be sure to take advantage of the customer support available to all ANSYS Fluent users.

.. Steps in Solving Your CFD Problem

.. Planning Your CFD Analysis

Once you have determined the important features of the problem you want to solve, follow the basic

procedural steps shown below.

. Define the modeling goals.

. Create the model geometry and mesh.

. Set up the solver and physical models.

. Compute and monitor the solution.

. Examine and save the results.

. Consider revisions to the numerical or physical model parameters, if necessary.

Step . of the solution process requires a geometry modeler and mesh generator. You can use Design-

Modeler and ANSYS Meshing within ANSYS Workbench or you can use a separate CAD system for

geometry modeling and mesh generation. When meshing 3D geometries, you can also use the meshing

mode of Fluent. Alternatively, you can use supported CAD packages to generate volume meshes for

import into ANSYS Fluent (see the User's Guide (p. )). For more information on creating geometry

and generating meshes using each of these programs, refer to their respective manuals.

The details of the remaining steps are covered in the User's Guide (p. ).

For each of the problem-solving steps, there are some questions that you need to consider:

Defining the Modeling Goals

– What results are you looking for, and how will they be used?

→ What are your modeling options?

→ What physical models will need to be included in your analysis?

→ What simplifying assumptions do you have to make?

→ What simplifying assumptions can you make?

→ Do you require a unique modeling capability?

Could you use user-defined functions (written in C)?

– What degree of accuracy is required?

– How quickly do you need the results?

– How will you isolate a piece of the complete physical system?

– Where will the computational domain begin and end?

→ Do you have boundary condition information at these boundaries?

→ Can the boundary condition types accommodate that information?

→ Can you extend the domain to a point where reasonable data exists?

– Can it be simplified or approximated as a 2D or axisymmetric problem?

Creating Your Model Geometry and Mesh

ANSYS Fluent uses unstructured meshes in order to reduce the amount of time you spend generating

meshes, to simplify the geometry modeling and mesh generation process, to enable modeling of

more complex geometries than you can handle with conventional, multi-block structured meshes,

and to enable you to adapt the mesh to resolve the flow-field features. ANSYS Fluent can also use

body-fitted, block-structured meshes (for example, those used by ANSYS Fluent  and many other

CFD solvers). ANSYS Fluent is capable of handling triangular and quadrilateral elements (or a combin-

ation of the two) in 2D, and tetrahedral, hexahedral, pyramid, wedge, and polyhedral elements (or a

combination of these) in 3D. This flexibility enables you to pick mesh topologies that are best suited

for your particular application, as described in the User's Guide (p. ).

For 3D geometries, you can create the mesh using the meshing mode of Fluent; otherwise, you must

generate the initial mesh (whatever the element types used) outside of Fluent or use one of the CAD

systems for which mesh import filters exist. When in solution mode, Fluent can be used to adapt all

types of meshes (except for polyhedral), in order to resolve large gradients in the flow field.

The following questions should be considered when you are generating a mesh:

– Can you benefit from other ANSYS, Inc. products such as CFX or ANSYS Icepak?

– Can you use a quad/hex mesh or should you use a tri/tet mesh or a hybrid mesh?

→ How complex is the geometry and flow?

→ Will you need a non-conformal interface?

– What degree of mesh resolution is required in each region of the domain?

→ Is the resolution sufficient for the geometry?

Basic Steps for CFD Analysis using ANSYS Fluent

→ Can you predict regions with high gradients?

→ Will you use adaption to add resolution?

– Do you have sufficient computer memory?

→ How many cells are required?

→ How many models will be used?

Setting Up the Solver and Physical Models

For a given problem, you will need to:

– Import and check the mesh.

– Select the numerical solver (for example, density based, pressure based, unsteady, and so on).

– Select appropriate physical models.

→ Turbulence, combustion, multiphase, and so on.

– Define material properties.

→ Fluid

→ Solid

→ Mixture

– Prescribe operating conditions.

→ Fluid

→ Solid

→ Mixture

– Prescribe boundary conditions at all boundary zones.

– Provide an initial solution.

– Set up solver controls.

– Set up convergence monitors.

– Initialize the flow field.

Computing and Monitoring Your Solution

– The discretized conservation equations are solved iteratively.

→ A number of iterations are usually required to reach a converged solution.

– Convergence is reached when:

→ Changes in solution variables from one iteration to the next are negligible.

Residuals provide a mechanism to help monitor this trend.

→ Overall property conservation is achieved.

Planning Your CFD Analysis

– The accuracy of a converged solution is dependent upon:

→ Appropriateness and accuracy of physical models.

→ Mesh resolution and independence.

→ Problem setup.

Examining and Saving Your Results

Examine the results to review the solution and extract useful data.

– Visualization tools can be used to answer such questions as:

→ What is the overall flow pattern?

→ Is there separation?

→ Where do shocks, shear layers, and so on form?

→ Are key flow features being resolved?

– Numerical reporting tools can be used to calculate the following quantitative results:

→ Forces and moments

→ Average heat transfer coefficients

→ Surface and volume integrated quantities

→ Flux balances

Revising Your Model

Once your solution is converged, the following questions should be considered when you are analyzing

the solution:

– Are physical models appropriate?

→ Is flow turbulent?

→ Is flow unsteady?

→ Are there compressibility effects?

→ Are there 3D effects?

– Are boundary conditions correct?

→ Is the computational domain large enough?

→ Are boundary conditions appropriate?

→ Are boundary values reasonable?

– Is the mesh adequate?

→ Can the mesh be adapted to improve results?

→ Does the solution change significantly with adaption, or is the solution mesh independent?

→ Does boundary resolution need to be improved?

Chapter : Guide to a Successful Simulation Using ANSYS Fluent

The following guidelines can help you make sure your CFD simulation is a success. Before logging a

technical support request, make sure you do the following:

. Examine the quality of the mesh in Fluent.

There are two basic things that you should do before you start a simulation:

Perform a mesh check to avoid problems due to incorrect mesh connectivity, and so on. In particular,

you should be sure that the minimum reported cell volume is not negative.

Look at maximum cell skewness (for example, using the Compute button in the Contours dialog box

after initializing the model). As a rule of thumb, the skewness should be below ..You can also use

the Report Quality function to calculate the minimum cell orthogonality.You can find more details

about mesh quality considerations in Mesh Quality in the Fluent User's Guide (p. ).

If there are mesh problems, you may have to re-mesh the problem.

. Scale the mesh and check length units.

In ANSYS Fluent, all physical dimensions are initially assumed to be in meters. You should scale the

mesh accordingly. Other quantities can also be scaled independently of other units used. ANSYS

Fluent defaults to SI units.

. Employ the appropriate physical models.

. Set the energy under-relaxation factor between . and .

For problems with conjugate heat transfer, when the conductivity ratio is very high, smaller values

of the energy under-relaxation factor practically stall the convergence rate.

. Use node-based gradients with unstructured tetrahedral meshes.

The node-based averaging scheme is known to be more accurate than the default cell-based scheme

for unstructured meshes, most notably for triangular and tetrahedral meshes.

. Monitor convergence with residuals history.

Residual plots can show when the residual values have reached the specified tolerance. After the

simulation, note if your residuals have decreased by at least  orders of magnitude to at least

.

For the pressure-based solver, the scaled energy residual must decrease to

. Also, the scaled

species residual may need to decrease to

to achieve species balance.

You can also monitor lift, drag, or moment forces as well as pertinent variables or functions (for

example, surface integrals) at a boundary or any defined surface.

. Run the CFD simulation using second order discretization for better accuracy rather than a faster solution.

A converged solution is not necessarily a correct one. You should use the second-order upwind

discretization scheme for final results.

. Monitor values of solution variables to make sure that any changes in the solution variables from one iter-

ation to the next are negligible.

. Verify that property conservation is satisfied.

After the simulation, note if overall property conservation has been achieved. In addition to monit-

oring residual and variable histories, you should also check for overall heat and mass balances. At

a minimum, the net imbalance should be less than % of the smallest flux through the domain

boundary.

. Check for mesh dependence.

You should ensure that the solution is mesh-independent and use mesh adaption to modify the

mesh or create additional meshes for the mesh-independence study.

. Check to see that the solution makes sense based on engineering judgment.

If flow features do not seem reasonable, you should reconsider your physical models and boundary

conditions. Reconsider the choice of the boundary locations (or the domain). An inadequate choice

of domain (especially the outlet boundary) can significantly impact solution accuracy.

You are encouraged to collaborate with your technical support engineer in order to develop a solution

process that ensures good results for your specific application. This type of collaboration is a good in-

vestment of time for both yourself and the ANSYS Fluent support engineer.

Guide to a Successful Simulation Using ANSYS Fluent

Chapter : Starting and Executing ANSYS Fluent

This chapter provides instructions for starting and executing ANSYS Fluent.

.. Starting ANSYS Fluent

.. Running ANSYS Fluent in Batch Mode

.. Switching Between Meshing and Solution Modes

.. Checkpointing an ANSYS Fluent Simulation

.. Cleaning Up Processes From an ANSYS Fluent Simulation

.. Exiting ANSYS Fluent

The following sections describe how start ANSYS Fluent:

... Starting ANSYS Fluent Using Fluent Launcher

... Starting ANSYS Fluent on a Windows System

... Starting ANSYS Fluent on a Linux System

... Command Line Startup Options

You can interactively specify ANSYS Fluent dimension, display, processing and other options using the

Fluent Launcher.

To start the Fluent Launcher, do one of the following:

Start ANSYS Fluent from the Linux or Windows command line with no arguments.

Start ANSYS Fluent from the Windows Start menu.

Start ANSYS Fluent from the Windows desktop or Quick Launch bar.

Any options set in the Fluent Launcher will be retained for your next session.

Specify the Dimension of the simulation you intend to perform.

Important

For Meshing Mode, you must select 3D. Meshing Mode is not available if 2D is selected.

Select your required Display Options.

Optionally, choose to Display Mesh After Reading (disabled by default).This option is applicable only to

volume meshes and not surface meshes. All of the boundary zones will be displayed except for the interior

zones of 3D geometries.

Note

You can override this option on a file-by-file basis using the Display Mesh After Reading

option in the Select File dialog box that opens when you are reading in a file.

Starting and Executing ANSYS Fluent

Optionally, enable the Load ACT option to load ANSYS ACT. For additional information on ACT, see

Customizing Fluent in the Fluent User's Guide (p. ).

Select your required Options.

Choose to perform solution calculations in Double-Precision mode, if desired. (Default is single-precision

mode) See Single-Precision and Double-Precision Solvers (p. ) to help with your decision.

Note

Meshing Mode is always run in Double Precision. This option applies for Solution Mode

only.

Choose to start ANSYS Fluent in Meshing Mode, if desired. (Default is Solution Mode.) See the Fluent User’s

Guide (p. ) for further details about using Fluent in meshing mode.

Choose an appropriate Use Job Scheduler option, if applicable. For example, the Microsoft Job Scheduler

for Windows, or LSF, SGE, and PBS Pro on Linux. For more information about using Fluent Launcher with

job schedulers, see Setting Scheduler Options in Fluent Launcher (p. ), as well as Setting Parallel Scheduler

Options in Fluent Launcher (p. ) in the User's Guide (p. ).

Note

This option is available only if Parallel is selected under Processing Options.

You can choose to run parallel simulations on Linux clusters, via the Windows interface using the Use Remote

Linux Nodes option (see Setting Remote Options in Fluent Launcher (p. ) for details).

Note

Select your required Processing Options.

Use Serial to restrict the meshing/solution calculations to a single processor core.

Use Parallel to allow multiple simultaneous processes.You will be asked to specify the number of

processes for both Meshing (if enabled) and Solver. See Setting Parallel Options in Fluent Launch-

er (p. ).When parallel is enabled, several additional parallel-specific items are available for selection

in the Parallel ribbon tab.

Select Show More Options to expand the Fluent Launcher window to reveal more options. (Fig-

ure . : The General Options Tab of Fluent Launcher (p. )). Note that once Fluent Launcher expands,

Starting ANSYS Fluent

the Show More Options button becomes the Show Fewer Options button, allowing you to hide the

additional options.

Important

Fluent Launcher also appears when you start ANSYS Fluent within ANSYS Workbench. For

more information, see the separate ANSYS Fluent in Workbench User's Guide.

.... Setting General Options in Fluent Launcher

Set file and path options using the General Options tab in Fluent Launcher.

Figure . : The General Options Tab of Fluent Launcher

.

Enable Pre/Post Only to run ANSYS Fluent with only the setup and postprocessing capabilities available.

The default ANSYS Fluent full solution mode allows you to set up, solve, and postprocess a problem,

while Pre/Post Only will not allow you to perform calculations.

.

Specify the path of your current working directory using the Working Directory field or click

to

browse through your directory structure.

Note

a Uniform Naming Convention (UNC) path cannot be set as a working directory. You

need to map a drive to the UNC path (Windows only)

.

Specify the location of the ANSYS Fluent installation on your system using the Fluent Root Path field,

or click

.

or click

to browse through your directory structure.Try to use the UNC path if applicable.

Note

The

button automatically converts a local path to a UNC path if any matching

shared directory is found (Windows only). Once set, various fields in Fluent Launcher (for

example, parallel settings, etc.) are automatically populated with the available options,

depending on the ANSYS Fluent installations that are available.

.

To use a journal file to automatically load the case, compile any user-defined functions, iterate until the

solution converges, and write results to an output file,

a.

Enable Use Journal File.

Note

This option does not support reading multiple journal files.

b.

Specify your journal file path and name, or click

to browse through your directory structure

to locate the file.

.... Single-Precision and Double-Precision Solvers

Both single-precision and double-precision versions of ANSYS Fluent are available on all computer

platforms. For most cases, the single-precision solver will be sufficiently accurate, but certain types

of problems may benefit from the use of a double-precision version. Several examples are listed below:

If your geometry has features of very disparate length scales (for example, a very long, thin pipe), single-

precision calculations may not be adequate. Note that nodal coordinates are always stored in double

precision (even for the single-precision version of ANSYS Fluent), so they are not a concern in this regard.

If your geometry involves multiple enclosures connected via small-diameter pipes (for example, automotive

manifolds), mean pressure levels in all but one of the zones can be quite large (since you can set only one

global reference pressure location). Double-precision calculations may therefore be necessary to resolve

the pressure differences that drive the flow, since these will typically be much smaller than the pressure

levels.

For conjugate problems involving high thermal-conductivity ratios and/or high-aspect-ratio meshes,

convergence and/or accuracy may be impaired with the single-precision solver, due to inefficient transfer

of boundary information.

For multiphase problems where the population balance model is used to resolve particle size distributions,

which could have statistical moments whose values span many orders of magnitude.

Note

ANSYS Fluent allows only a period to be used as a decimal separator. If your system is set

to a European locale that uses a comma separator (for example, Germany), fields that accept

numeric input may accept a comma, but may ignore everything after the comma. If your

system is set to a non-European locale, numeric fields will not accept a comma at all.

ANSYS Workbench accepts commas as decimal delimiters. These are translated into periods

when data is passed to ANSYS Fluent.

.... Setting Parallel Options in Fluent Launcher

The Parallel Settings tab allows you to specify settings for running ANSYS Fluent in parallel. This tab

is only available if you have selected Parallel under Processing Options.

Figure . : The Parallel Settings Tab of Fluent Launcher

Once you select Parallel,

.

.

Enter the number of processes to be used for meshing under Meshing Processes, if enabled.

.

Enter the number of processes to be used for solution under Solver Processes.When you change to

solution mode, additional processes will be spawned as necessary to bring the total number of processes

to this value.This must be set to a value greater than or equal to Meshing Processes.

.

If your machine is equipped with General Purpose Graphics Processing Units you can also specify GPGPUs

per Machine.

Note

With Parallel processing enabled, some global file read and write operations are affected.

Unavailable options will have their menu entry grayed out.

Refer to Parallel Processing in the Fluent User's Guide (p. ) for details on parallel processing using

Fluent and Starting Parallel ANSYS Fluent Using Fluent Launcher in the Fluent User's Guide (p. ) for

additional details parallel process configuration options on this tab.

.... Setting Remote Options in Fluent Launcher

The Remote tab (Figure . : The Remote Tab of Fluent Launcher (p. )) allows you to specify settings

for running ANSYS Fluent parallel simulations on Linux clusters, via the Windows interface.

Figure . : The Remote Tab of Fluent Launcher

For additional information about this tab, see Setting Additional Options When Running on Remote

Linux Machines (p. ) in the User's Guide (p. ).

.... Setting Scheduler Options in Fluent Launcher

The Scheduler tab (Figure . : The Scheduler Tab of Fluent Launcher (Windows  Version) (p. ))

allows you to specify settings for running ANSYS Fluent with various job schedulers (for example, the

Microsoft Job Scheduler for Windows, or LSF, SGE, and PBS Pro on Linux). This tab is available if you

have selected Use Job Scheduler under Options.

Figure . : The Scheduler Tab of Fluent Launcher (Windows  Version)

For additional information about this tab, see Setting Parallel Scheduler Options in Fluent Launch-

er (p. ) in the User's Guide (p. ).

.... Setting Environment Options in Fluent Launcher

The Environment tab (Figure . : The Environment Tab of Fluent Launcher (p. )) allows you to

specify compiler settings for compiling user-defined functions (UDFs) with ANSYS Fluent (Windows

only). The Environment tab also allows you to specify environment variable settings for running

ANSYS Fluent.

Figure . : The Environment Tab of Fluent Launcher

Specify a batch file that contains UDF compilation environment settings by selecting the Set up

Compilation Environment for UDF check box (enabled by default). Once selected, you can then

enter a batch file name in the text field. By default, Fluent Launcher uses the udf.bat file that is

located in the directory where ANSYS Fluent is installed. It is recommended that you keep the default

batch file, which is tested with the three most recent versions of MS Visual Studio C++ compilers at

the time of the ANSYS Fluent release date (as noted in Compiler Requirements for Windows Systems).

For more information about compiling UDFs, see the separate Fluent Customization Manual.

Under Other Environment Variables, enter or edit license file or environment variable information

in the text field. For example, FLUENT_AFFINITY=x specifies the process binding (affinity) setting,

in the same manner as the -affinity=x command line option (see Parallel Options (p. ) for

details). Using the Default button resets the default value(s).

There are two ways to start ANSYS Fluent on a Windows system:

From the Windows Start menu, click Start > ANSYS  R3 > Fluid Dynamics > Fluent  R3

This option starts Fluent Launcher (see Starting ANSYS Fluent Using Fluent Launcher (p. )). The

Fluent Launcher may also be accessed via an icon on your desktop or in the Quick Launch bar.

Note

If the default “ANSYS  R3” program group name was changed when ANSYS Fluent was

installed, you will find the Fluent menu item in the program group with the new name

that was assigned, rather than in the ANSYS  R3 program group.

From a Command Prompt window, type fluent version, where version is replaced with one of the

four options specifying the dimension and precision of the solver.

– 2d for the 2D, single-precision solver.

– 3d for the 3D, single-precision solver.

– 2ddp for the 2D, double-precision solver.

– 3ddp for the 3D double-precision solver.

For additional information on starting Fluent from the command prompt, see Command Line Startup

Options (p. ).

Important

To be able to start ANSYS Fluent from the command prompt, be sure the path to your

ANSYS Fluent home directory is in your command search path environment variable by

Important

executing the setenv.exe program located in the ANSYS Fluent directory (for example,

C:\Program Files\ANSYS Inc\v195\fluent\ntbin\win64).

Tip

You can also start the parallel version of ANSYS Fluent, or start ANSYS Fluent in meshing

mode from the Command Prompt.

To start the parallel version on x processors, type fluent version -tx, replacing version

with the desired solver version and x with the number of processors. For example, fluent

3d -t4 to run the 3D version on  processors.

To start in meshing mode, add the command line option -meshing. For example, fluent

3d -meshing to start in meshing mode.

Both parallel and meshing mode may be combined.You must specify the number of meshing

processes using -tmy. For example, fluent 3ddp -meshing -tm4 -t8 will start ANSYS

Fluent in meshing mode with  meshing processes.When switched to solution mode, the

solver will be 3D, double precision and run  processes.

There are two ways to start ANSYS Fluent on a Linux system:

Start Fluent from the command line without specifying a version, and then use Fluent Launcher to choose

the appropriate version along with other options. See Starting ANSYS Fluent Using Fluent Launcher (p. )

for details.

Start the appropriate version from the command line by typing fluent version, where version is

replaced with one of the four options specifying the dimension and precision of the solver.

You can also start the parallel version of ANSYS Fluent from the command line. To start the parallel

version on x processors, type fluent version -tx at the prompt, replacing version with the

desired solver version and x with the number of processors. For example, fluent 3d -t4 will run

the 3D version on  processors. See Starting Parallel ANSYS Fluent on a Linux System (p. ) in the

User's Guide (p. ) for more information about starting the parallel solvers.

Note

ANSYS Fluent automatically selects the best graphics driver and defaults to the X11 driver

when it does not detect the required graphics support. You can use the HOOPS_PICTURE

environment variable to force a particular graphics driver, if you feel it is necessary to use

an alternate driver.

Table . : Available Command Line Options for Linux and Windows Platforms (p. ) lists the available

command line arguments for Linux and Windows. More detailed descriptions of these options can be

found in the following sections.

To obtain information about available startup options, you can type fluent -help before starting

up Fluent.

Table . : Available Command Line Options for Linux and Windows Platforms

Description

Platform

Option

Start Fluent in server mode.

all

aas

Load ACT on Fluent startup.

all

act

Specifies the process binding (affinity)

setting, as described in Parallel

all

affinity=<x>

Loads the specified application, for

example flremote launches the

Remote Visualization Client.

all

app=<x>

Runs the specified script in the

all

all

app=<x>

specified application (must be used

with the -app=<x> startup option.

all

appscript=<scriptfile>

Uses the Microsoft Job Scheduler,

where <x> is the head node name.

Windows only

ccp <x>

Ensures that the file cache buffers are

flushed.

Linux only

cflush

Specifies that <x> is the hosts file or

(for Linux) machine list.

all

cnf=<x>

Sets the graphics driver (available

drivers vary by platform, and include

all

driver <name>

opengl, x11, and null for Linux and

opengl, msw, and null for Windows).

Show environment variables.

all

env

Run without the GUI or graphics.

all

g

Specifies the number of GPGPUs per

machine that should be used for AMG

acceleration. Only available in parallel.

Linux and Win64

only

gpgpu=<n>

Run without graphics.

all

gr

Run without the GUI but with graphics.

You cannot interact with the displayed

graphics objects.

all

gu

Platform

Option

Specifies that <hostname> is used for

running Cortex (the process that

manages the GUI and graphics).

Linux only

gui_machine=<hostname>

Display command line options.

all

help

Run in minimized mode.

hidden

Specifies that the IP interface

<host:ip> is to be used by the host.

all

host_ip=<host:ip>

Reads the specified journal file(s). Read

multiple journals at once as follows: -i

all

i <journal>

example1.jou -i example2.jou

i example3.jou ... AAS Mode

does not support multiple journals from

the command line.

Start Fluent in meshing mode (you

must specify Fluent as either 3d or

3ddp).

all

meshing

3ddp).

all

meshing

Specifies that the MPI implementation

is ibmmpi|intel|....

all

mpi=<mpi>

Launches an MPI program to collect

network performance data and prints

all

mpitest

to console (Linux) or to the working

directory (Windows).

Do not display mesh after reading.

all

nm

Specify interconnect; <ic>={default

| eth | ib}

all

p<ic>

Check the network connections before

spawning compute nodes.

Linux only

pcheck

Loads a binary that is specially ported

for a particular platform, as described

in Performance Options (p. ).

Linux only

platform=<x>

Run the ANSYS Fluent

postprocessing-only executable.

all

post

List all releases installed in the current

directory.

all

r

Run release <x> of ANSYS Fluent.

all

r<x>

Specify the machine to be used for

executing mpirun to launch the node

Linux only

remote_node=<hostname>

processes; if =<hostname> is omitted,

the first node in the hosts file will be

used.

Run ANSYS Fluent under a scheduler;

<scheduler> can be set to lsf

Linux only

scheduler=<scheduler>

(LSF), pbs (PBS Professional), or sge

(Univa Grid Engine—formerly Sun Grid

Engine).

Platform

Option

Enables an additional option <opt>

that is relevant for the selected

Linux only

scheduler_opt=<opt>

scheduler; this command line option

can be included multiple times.

Sets the parallel environment to <pe>

when running under SGE.

Linux only

scheduler_pe=<pe>

Sets the scheduler queue to <queue>.

Linux only

scheduler_queue=<queue>

Enables a job-scheduler-supported

native remote node access mechanism.

Linux only

Linux only

Linux only

Linux only

scheduler_tight_coupling

Sets the environment variable <var>

to <value>.

all

setenv="<var>=<value>"

Run ANSYS Fluent and start the remote

visualization server. You can provide a

all

sifile=<name>.txt

path before the server info filename to

specify where the file is created.

Prints the memory bandwidth.

Linux only

stream

Specifies that the number of processors

is <x>.

all

t<x>

for meshing is <x>.

all

tm<x>

.... ACT Option

fluent -act loads ANSYS ACT at Fluent startup. For additional information about ACT in Fluent,

see Customizing Fluent in the Fluent User's Guide (p. ).

.... Application Option

fluent -app, when set equal to flremote, launches either the Fluent Launcher or the specified

dimension of Fluent (for example, 3ddp), along with the Fluent Remote Visualization Client. For addi-

tional information about the Fluent Remote Visualization Client, refer to Remote Visualization and

Accessing Fluent Remotely (p. ).

.... Application Script Option

fluent -appscript, allows you to specify a script that will run in the specified application

(-appscript must be used in conjunction with -app).

.... Graphics Options

Note

Fluent automatically selects the best graphics driver for the given runtime environment,

unless you choose a specific graphics driver with the fluent -driver command line

option.

fluent -driver allows you to specify the graphics driver to be used in the session. When enabling

option.

graphics display, you have various options: on Linux, the available drivers include fluent -driver

opengl and fluent -driver x11; on Windows, the available drivers include fluent -driver

opengl and fluent -driver msw (the latter instructs ANSYS Fluent to use the Operating Systems

Windows driver). For both Linux and Windows, you can disable graphics display using fluent -

driver null. For a comprehensive list of the drivers available to you, open a Fluent session, enter

the display/set/rendering-options/driver text command, and then press the Enter key

at the driver> prompt. For more details about using the driver options, see Hiding the Graphics

Window Display (p. ) in the User's Guide (p. ).

Note

For any session that displays graphics in a graphics window and/or saves picture files,

having the driver set to x11, msw, or null will cause the rendering / saving speed to be

significantly slower.

fluent -gui_machine=<hostname> will run Cortex on a specified machine (<hostname>).

This option is only available when running on Linux, and may be needed to ensure optimal graphics

performance when running Fluent under a scheduler / load manager (using the -scheduler=<sched-

uler> option, as described in Scheduler Options (p. )).

Important

(Exceed onDemand Only) When you are using the -gui_machine flag you must also use

setenv="CORTEX_PRE=ssrun" to specify the server side rendering to ensure accel-

erated graphics performance.

For example: fluent 3ddp -t2 -setenv="CORTEX_PRE=/opt/Exceed_connec-

tion_server_13.8_64/bin/ssrun" -scheduler=<scheduler> -sched-

uler_queue=<queue> -gui_machine=<hostname>

Note that the path to ssrun may be different for your specific environment.

fluent -g will run Cortex without graphics and without the graphical user interface. This option

is useful if want to submit a batch job.

fluent -gr will run Cortex without graphics. This option can be used in conjunction with the -i

<journal> option to run a job in “background” mode.

fluent -gu will run Cortex without the graphical user interface but will open graphics windows

and display graphics objects. You cannot interact with the displayed graphics objects.

To start Fluent and immediately read a journal file, type fluent -i <journal>, replacing

<journal> with the name of the journal file you want to read.

fluent -nm will run Cortex without displaying the mesh in the graphics window.

Important

Download graphics card driver updates directly from the graphics card vendor's website,

for example www.nvidia.com. Do not use the "Update Driver" feature offered by the oper-

ating system as these can sometimes update to an older version of the driver.

.... Meshing Mode Option

fluent -meshing specifies that Fluent opens in meshing mode rather than the default solution

mode. See the Fluent User’s Guide (p. ) for further details about the meshing mode.

.... Performance Options

cflush specifies that memory is allocated in such a way as to ensure that all of the associated file

cache buffers are flushed. This may resolve processing performance issues. For more details, see

Clearing the Linux File Cache Buffers (p. ) in the User's Guide (p. ).

platform=<x> loads a binary that is specially ported for a particular platform. When <x>=intel,

an AVX2 optimized binary is used that enhances performance when running on processors that

support the AVX2 instruction set (available only on Linux).

stream prints the memory bandwidth, using a variant of the STREAM benchmark. This information

can be helpful in determining if your memory is set up in an optimal manner.

.... Parallel Options

These options are used in association with the parallel solver.

affinity=<x> specifies the process binding (affinity) setting, except when the Microsoft MPI is

used in Windows—in that case, the Microsoft MPI affinity setting is always used; for all other cases,

process binding is enabled by default and can be disabled by setting <x>=off (except when the

Intel MPI is used on Windows, in which case the Intel MPI affinity setting is used). When running on

Linux in exclusive mode (that is, when no other users / jobs have access to your machine) or on

Windows, Fluent will assign the processes in an optimized manner when process binding is enabled.

When running on Linux in non-exclusive mode, you can set the affinity thusly: when <x>=sock (the

default), processes are bound to a core if no other jobs are running on the machine, otherwise they

are bound to a socket; when <x>=core, processes are bound to a core in all cases.

ccp <x> (where <x> is the name of the head node) runs the parallel job through the Microsoft

Job Scheduler as described in Starting Parallel ANSYS Fluent with the Microsoft Job Scheduler (p. )

in the User's Guide (p. ).

cnf=<x> (where <x> is the name of a hosts file or a list of Linux machines) spawns a compute

node on each of the specified machines. For details, see Starting Parallel ANSYS Fluent on a Windows

System Using Command Line Options (p. ) or Starting Parallel ANSYS Fluent on a Linux System

Using Command Line Options (p. ) in the User's Guide (p. ).

gpgpu=<n> specifies the number of general purpose graphics processing units (GPGPUs) per machine

to be used for AMG acceleration. For more information, see Using General Purpose Graphics Processing

Units (GPGPUs) With the Algebraic Multigrid (AMG) Solver in the Fluent User's Guide (p. ).

host_ip=<host:ip> specifies the IP interface to be used by the host process.

mpi=<mpi> specifies that <mpi> is to be used for the MPI. You can skip this flag if you choose to

use the default MPI.

mpiopt=<x> allows you to specify any additional MPI flags (<x>) to be included in the run (Linux

only).

mpitest runs the mpitest program instead of ANSYS Fluent to test the network.

p<ic> specifies the use of parallel interconnect <ic>, where <ic> can be any of the interconnects

listed in Starting Parallel ANSYS Fluent on a Windows System Using Command Line Options (p. )

or Starting Parallel ANSYS Fluent on a Linux System Using Command Line Options (p. ) in the User's

Guide (p. ).

pcheck checks the network connections before spawning compute nodes (Linux only).

By default, the mpirun command (which launches the node processes) is executed on the compute

node where the host process is spawned. You can use -remote_node=<hostname> to specify a

different machine for the execution of this command. If =<hostname> is omitted, the first node in

the hosts file will be used. (Linux only)

ssh specifies that SSH should be used to spawn remote processes. (Beginning with ANSYS Fluent

R16., SSH is used by default. This option is included primarily for backward compatibility with existing

launch scripts, etc.)

t<x> specifies that <x> processors are to be used. For more information about starting the parallel

version of ANSYS Fluent, see Starting Parallel ANSYS Fluent on a Windows System (p. ) or Starting

Parallel ANSYS Fluent on a Linux System (p. ) in the User's Guide (p. ).

tm<x> specifies that <x> processors are to be used for meshing. This value must be less than or

equal to the number of processes specified with -t<x>.

.... Postprocessing Option

fluent -post will run a version of Fluent that allows you to set up a problem or perform postpro-

cessing, but will not allow you to perform calculations. Running ANSYS Fluent for pre- and postpro-

cessing requires you to use the -post flag on startup. To use this option on Linux, launch ANSYS

Fluent by adding the -post flag after the version number, for example,

fluent 3d -post

To use this same feature from the graphical interface on Windows or Linux, select the Pre/Post option

in the General tab of Fluent Launcher, as described in Starting ANSYS Fluent Using Fluent Launch-

er (p. ).

.... Remote Visualization Options

The -sifile=<name>.txt option starts ANSYS Fluent and the server that is necessary for running

er (p. ).

the remote visualization client. For additional information on remote visualization, refer to Remote

Visualization and Accessing Fluent Remotely (p. ).

Note

You can specify the location for the server info file prior to the filename, for example

sifile=D:/example_folder/server_info_example_name.txt. If you do not

provide a file path before the file name and you do not provide a path using the SERV-

ER_INFO_DIR environment variable, then the file is saved in your working directory.

.... Scheduler Options

The -scheduler=<scheduler> option allows you to specify that your Linux session is run under

a scheduler / load manager, where <scheduler> can be one of the following:

lsf: this allows you to run ANSYS Fluent under IBM Spectrum LSF software, and thereby take advantage

of the checkpointing features of that load management tool. For further details, see Part I: Running Fluent

Under LSF.

pbs: this runs ANSYS Fluent under Altair PBS Professional, and allows you to use the features of this software

to manage your distributed computing resources. For further details, see Part II: Running Fluent Under

PBS Professional.

sge: this runs ANSYS Fluent under Univa Grid Engine (previously known as Sun Grid Engine, or

SGE) software, and allows you to use the features of this software to manage your distributed

computing resources. For further details, see Part III: Running Fluent Under SGE.

Note

You can use the -scheduler=<scheduler> option along with the -gui_ma-

chine=<hostname> (described in Graphics Options (p. )), in order to ensure optimal

graphics performance.

Note

Other options are available when you use a scheduler: you can specify a queue using -sched-

uler_queue=<queue>; you can enable an additional option for the scheduler using -sched-

uler_opt=<opt> (note that you can include multiple instances of this option when you want to

use more than one scheduler option); and when running under Univa Grid Engine software, you can

set the parallel environment using -scheduler_pe=<pe>.

It is also possible to enable a job-scheduler-supported native remote node access mechanism using

scheduler_tight_coupling in Linux. For details about the MPI / job scheduler combinations

that are supported for this tight coupling, see Running Fluent Using a Load Manager.

....Version, Release Options, and Environment Variables

Typing fluent <version> -r, replacing <version> with the desired version (2d or 3d, or for

double precision, fluent  or 3ddp), will list all releases of the specified version.

fluent -r<x> will run release <x> of ANSYS Fluent.

Typing fluent <version> -env, replacing <version> with the desired version, will list all

environment variables before running ANSYS Fluent.

Including the -setenv="<var>=<value>" option sets the environment variable <var> explicitly

to <value> before launching ANSYS Fluent. Note that you can include as many instances of this

option as you need to set all of the relevant environment variables. You can also unset an environment

variable by entering -setenv="<var>=".

.... System Coupling Options

The following command line options (in either Windows or Linux) can be used when ANSYS Fluent

is involved in a system coupling simulation.

schost="<x>" (where <x> is the name of the host machine, in quotes) specifies the host machine

on which the coupling service is running (to which the co-simulation participant/solver must connect).

scid=<y> (where <y> is the session-id of the system coupling run, without quotes) specifies the

identity of the coupling service run.

sclic=<x> (where <x> is the name of the port and host machine, without quotes) specifies the

port and host of the machine with the system coupling license running (that the co-simulation parti-

cipant/solver must connect to). For example, @localhost.

scport=<y> (where <y> is the port number) specifies the port on the host machine upon which

the coupling service is listening for connections from co-simulation participants.

scname="<z>" (where <z> is the name of the participant, in quotes) specifies the unique name

used by the co-simulation participant to identify itself to the coupling service (see System Coupling

Server File (scServer.scs) in the System Coupling User's Guide for more information).

The general syntax for invoking ANSYS Fluent for system coupling is:

fluent 3d –schost=host name in quotes –scport=port number –scname=name of the solver

in quotes

For instance:

fluent 3d –schost="machine1.domain.com" –scport= –scname="Solution1"

Once ANSYS Fluent loads the case, initialize the solution using the following command:

s i i

Once your case is initialized, start the system coupling by typing the following command in the ANSYS

Fluent text user interface (TUI):

(sc-solve)

s i i

For more information, see Performing System Coupling Simulations Using Fluent (p. ) in the Fluent

User's Guide, as well as the System Coupling User's Guide.

.... Other Startup Options

There are other startup options that are not listed when you type the fluent -help command.

These options can be used to customize your graphical user interface. For example, to change the

ANSYS Fluent window size and position you can either modify the .Xdefaults file described in Modifying

the Graphical User Interface (p. ) in the User's Guide (p. ), or you can simply type the following

command at startup:

fluent <version> -geometry <XX>x<YY>+<xx>-<yy>

where <XX> and <YY> are the width and height in pixels, respectively, and +<xx>-<yy> is the pos-

ition of the window.

Therefore, typing fluent 3d -geometry 700x500+- will start the 3D version of ANSYS

Fluent, sizing the ANSYS Fluent console to 700x500 pixels and positioning it on your monitor screen

at +-.

There are additional Qt command line startup options for modifying the graphical stylesheet and

more, which can be found in Qt documentation.

ANSYS Fluent can be used interactively, with input from and display to your computer screen, or it can

be used in a batch or background mode in which inputs are obtained from and outputs are stored in

files. Generally you will perform problem setup, initial calculations, and postprocessing of results in an

interactive mode. However, when you are ready to perform a large number of iterative calculations,

you may want to run ANSYS Fluent in batch or background mode. This allows the computer resources

to be prioritized, enables you to control the process from a file (eliminating the need for you to be

present during the calculation), and also provides a record of the calculation history (residuals) in an

output file. While the procedures for running ANSYS Fluent in a batch mode differ depending on your

computer operating system, Background Execution on Linux Systems (p. ) provides guidance for

running in batch/background on Linux systems, and Background Execution on Windows Systems (p. )

provides guidance for running in batch/background on Windows systems.

For additional information, see the following sections:

... Background Execution on Linux Systems

... Background Execution on Windows Systems

... Batch Execution Options

To run ANSYS Fluent in the background in a C-shell (csh) on a Linux system, type a command of the

following form at the system-level prompt:

fluent 2d -g < inputfile > & outputfile &

or in a Bourne/Korn-shell, type:

fluent 2d -g < inputfile > outputfile >& &

In these examples,

Running ANSYS Fluent in Batch Mode

fluent is the command you type to run ANSYS Fluent interactively.

-g indicates that the program is to be run without the GUI or graphics (see Starting ANSYS Fluent (p. )).

inputfile is a file of ANSYS Fluent commands that are identical to those that you would type interactively.

outputfile is a file that the background job will create, which will contain the output that ANSYS Flu-

ent would normally print to the screen (for example, the menu prompts and residual reports).

& tells the Linux system to perform this task in background and to send all standard system errors (if any)

to outputfile.

The file inputfile can be a journal file created in an earlier ANSYS Fluent session, or it can be a file

that you have created using a text editor. In either case, the file must consist only of text interface

commands (since the GUI is disabled during batch execution). A typical inputfile is shown below:

; Read case file

rc example.cas

; Initialize the solution

/solve/initialize/initialize-flow

; Calculate  iterations

it

; Write data file

wd example50.dat

; Calculate another  iterations

it

; Write another data file

wd example100.dat

; Exit Fluent

exit

yes

This example file reads a case file example.cas, initializes the solution, and performs  iterations

in two groups of , saving a new data file after each  iterations. The final line of the file terminates

the session. Note that the example input file makes use of the standard aliases for reading and writing

case and data files and for iterating. (it is the alias for /solve/iterate, rc is the alias for

/file/read-case, wd is the alias for /file/write-data, etc.) These predefined aliases allow

you to execute commonly used commands without entering the text menu in which they are found.

In general, ANSYS Fluent assumes that input beginning with a / starts in the top-level text menu, so

if you use any text commands for which aliases do not exist, you must be sure to type in the complete

name of the command (for example, /solve/initialize/initialize-flow). Note also that

you can include comments in the file. As in the example above, comment lines must begin with a ;

(semicolon).

An alternate strategy for submitting your batch run, as follows, has the advantage that the outputfile

will contain a record of the commands in the inputfile. In this approach, you would submit the

batch job in a C-shell using:

fluent 2d -g -i inputfile  >& outputfile &

or in a Bourne/Korn-shell using:

fluent 2d -g -i inputfile > outputfile >& &

To run ANSYS Fluent in the background on a Windows system, the following commands can be used:

fluent 3d -g -i journal

fluent 3d -g -wait -i journal

fluent 3d -hidden -i journal

-g indicates that the program is to be run minimized in the task bar.

-i journal reads the specified journal file.

-wait is the command you type in a DOS batch file or some other script in a situation where the script

must wait until ANSYS Fluent has completed its run.

-hidden is similar to the -wait command, but also runs ANSYS Fluent completely hidden and non-inter-

actively.

To get an output (or transcript) file while running ANSYS Fluent in the background on a Windows

system, the journal file must contain the following command to write a transcript file:

; start transcript file

/file/start-transcript outputfile.trn

where the outputfile is a file that the background job will create, which will contain the output

that ANSYS Fluent would normally print to the screen (for example, the menu prompts and residual

reports).

See Creating and Reading Journal Files (p. ) in the User's Guide (p. ) for details about journal files.

See Creating Transcript Files (p. ) in the User's Guide (p. ) for details about transcript files.

During a typical session, ANSYS Fluent may require feedback from you in the event of a problem it

encounters. ANSYS Fluent usually communicates problems or questions through the use of Error dialog

boxes, Warning dialog boxes, or Question dialog boxes. While executing ANSYS Fluent in batch mode,

you may want to suppress this type of interaction in order to, for example, create journal files more

easily.

There are three common batch configuration options available to you when running ANSYS Fluent in

batch mode. You can access these options using the Batch Options dialog box (Figure . : The Batch

Options Dialog Box (p. )).

File → Batch Options...

Figure . : The Batch Options Dialog Box

The Batch Options dialog box contains the following items:

Confirm File Overwrite

determines whether ANSYS Fluent confirms a file overwrite.This option is turned on by default.

Hide Questions

allows you to hide Question dialog boxes.This option is turned off by default.

Exit on Error

allows you to automatically exit from batch mode when an error occurs.This option is disabled by default.

When run in batch mode through the command prompt or a journal file with Exit on Error enabled,

Fluent will exit under the following circumstances:

Normal run termination upon reaching the end of a journal (return value )

Error returned during scripted text command execution (return value )

Unexpected input (wrong type) to text command (return value )

Licensing error (return value )

If an invalid text command is entered, Fluent will not exit, but proceed to the next text input.

Note that in Windows you must start Fluent with the -wait command line option.

file → set-batch-options

Any combination of these options can be turned on or off at any given time prior to running in batch

mode.

Important

Batch option settings are not saved with case files. They are meant to apply for the duration

of the current ANSYS Fluent session only. If you read in additional mesh or case files during

this session, the batch option settings will not be altered. As batch options are not saved

with case files, journal files developed for use in batch mode should begin by enabling the

desired batch option settings (if different from the default settings).

You can switch from the meshing mode of Fluent to the solution mode by clicking the Switch to

Solution button, located by default in the top left corner of the application window. The mesh from

your meshing mode session will be transferred and read in the new solution mode session.

You can switch from the solution mode of Fluent to the meshing mode by using the switch-to-

meshing-mode text command. Note that this text command is only available for 3D sessions, before

you have read a mesh or case file.

The checkpointing feature of ANSYS Fluent allows you to save case and data files while your simulation

is running. While similar to the autosave feature of ANSYS Fluent (Automatic Saving of Case and Data

Files (p. ) in the User's Guide (p. )), which allows you to save files throughout a simulation, check-

pointing allows you slightly more control in that you can save an ANSYS Fluent job even after you have

started the job and did not set the autosave option. Checkpointing also allows you to save case and

data files and then exit out of ANSYS Fluent. This feature is especially useful when you need to stop an

ANSYS Fluent job abruptly and save its data.

There are two different ways to checkpoint an ANSYS Fluent simulation, depending upon how the

simulation has been started.

. ANSYS Fluent running under LSF or SGE

ANSYS Fluent is integrated with load management tools like LSF and SGE. These two tools allow

you to checkpoint any job running under them. You can use the standard method provided by

these tools to checkpoint the ANSYS Fluent job.

For more information on using ANSYS Fluent and SGE or LSF, see Part III: Running Fluent Under SGE

or Part I: Running Fluent Under LSF, respectively.

. Independently running ANSYS Fluent

When not using tools such as LSF or SGE, a different checkpointing mechanism can be used when

running an ANSYS Fluent simulation. You can checkpoint an ANSYS Fluent simulation while iterat-

ing/time-stepping, so that ANSYS Fluent saves the case and data files and then continues the calcu-

lation, or so that ANSYS Fluent saves the case and data files and then exits.

Saving case and data files and continuing the calculation:

On Linux, create a file called check-fluent, that is,

/tmp/check-fluent

On Windows, create a file called check-fluent.txt, that is,

C:\temp\check-fluent.txt

Saving case and data files and exiting ANSYS Fluent:

On Linux, create a file called exit-fluent, that is,

/tmp/exit-fluent

Checkpointing an ANSYS Fluent Simulation

On Windows, create a file called exit-fluent.txt, that is,

C:\temp\exit-fluent.txt

The saved case and data files will have the current iteration number appended to their file names.

ANSYS Fluent offers an alternate way to checkpoint an unsteady simulation. While the default beha-

vior is to checkpoint the simulation at the end of the current iteration, for unsteady simulations you

have the option of completing all of the iterations in the current time-step before checkpointing.

This can be set by entering the following Scheme command prior to running the unsteady simulation:

(ckpt/time-step? #t)

Now when you save the checkpoint file (as described previously), the case and data file will be saved

at the end of the current time step and named accordingly. To switch back to the default check-

pointing mechanism at the end of the current iteration, use the following Scheme command:

(ckpt/time-step? #f)

Important

Note that the (ckpt/time-step? #t) command will have the effect only in the case

of an unsteady simulation.

Note

Important

Note

It is recommended that you do not use checkpointing when using ANSYS Fluent in Workbench.

However, if checkpointing is necessary, the exit-fluent/exit-fluent.txt file can

be used and the file will be checked in its default location (the FFF/FLU system directory

containing the *.set file). If ANSYS Fluent is calculating, then the existence of the file is

equivalent to an interrupt command. Similarly, the check-fluent/check-fluent.txt

file can be used to save the project on demand when ANSYS Fluent is calculating.

ANSYS Fluent lets you easily remove extraneous processes in the event that an ANSYS Fluent simulation

must be stopped.

When a session is started, ANSYS Fluent creates a cleanup-fluent script file. The script can be used

to clean up all ANSYS Fluent-related processes. ANSYS Fluent creates the cleanup-script file in the current

working directory with a filename that includes the machine name and the process identification

number (PID) (for example, cleanup-fluent-mymachine-).

If the current directory does not possess the proper write permissions, then ANSYS Fluent will write the

cleanup-script file to your home directory.

If, for example, ANSYS Fluent is started on a machine called thor and the process identification number

is , ANSYS Fluent will create a cleanup-script called cleanup-fluent-thor- in the

current directory. To run the cleanup-script, and clean up all ANSYS Fluent processes related to your

session, on Linux platforms, type the following command in the console window:

sh cleanup-fluent-thor-

Or, if the shell script already has executable permissions, simply type:

cleanup-fluent-thor-

To clean up extraneous ANSYS Fluent processes on Windows (serial or parallel), double-click the corres-

ponding batch file (for example, cleanup-fluent-thor-.bat) that ANSYS Fluent generates

at the beginning of each session.

Important

During a normal run, this file will be deleted automatically after exiting ANSYS Fluent. In

abnormal situations, you may use this batch file to clean up the ANSYS Fluent processes.

Once an ANSYS Fluent session has been closed, you can safely delete any left over cleanup

scripts from your working directory.

Important

If an ANSYS Fluent session hangs or freezes on Windows, and you want to view the complete

contents of the ANSYS Fluent console output in a transcript file, you should use the taskkill

command through the DOS command prompt, rather than terminating the ANSYS Fluent

application through the Windows Task Manager.

You can exit ANSYS Fluent by selecting Exit in the File ribbon tab. If the present state of the program

has not been written to a file, a Question dialog box will open to confirm if you want to proceed. You

can cancel the exit and write the appropriate file(s) or you can continue to exit without saving the case

or data.

Exiting ANSYS Fluent

Glossary of Terms

This glossary contains a listing of terms commonly used throughout the documentation.

adaption (p. )

case files (p. )

cell types (p. )

computational fluid dynamics (CFD) (p. )

console (p. )

convergence (p. )

cortex (p. )

data files (p. )

dialog boxes (p. )

discretization (p. )

GUI (p. )

mesh (p. )

models (p. )

node (p. )

postprocessing (p. )

residuals (p. )

skewness (p. )

solvers (p. )

terminal emulator (p. )

TUI (p. )

adaption

A technique useful in improving overall mesh quality. The solution-adapt-

ive mesh refinement feature of ANSYS Fluent allows you to refine and/or

coarsen your mesh based on geometric and numerical solution data. In

addition, ANSYS Fluent provides tools for creating and viewing adaption

fields customized to particular applications.

case files

Files that contain the mesh, boundary conditions, and solution parameters

for a problem. A case file also contains the information about the user

interface and graphics environment.

cell types

The various shapes or units that constitute the base elements of a mesh.

ANSYS Fluent can use meshes composed of tetrahedral, hexahedral,

pyramid, wedge, or polyhedral cells (or a combination of these).

Figure : Cell Types

computational fluid dynam-

ics (CFD)

The science of predicting fluid flow, heat transfer, mass transfer (as in

perspiration or dissolution), phase change (as in freezing or boiling),

chemical reaction (for example, combustion), mechanical movement (for

example, fan rotation), stress or deformation of related solid structures

(such as a mast bending in the wind), and related phenomena by solving

the mathematical equations that govern these processes using a numer-

ical algorithm on a computer.

console

The console is part of the ANSYS Fluent application window that allows

for text command input and the display of information.

console

convergence

The point at which the solution is no longer changing with each success-

ive iteration. Convergence criteria, along with a reduction in residuals,

also help in determining when a solution is complete. Convergence cri-

teria are pre-set conditions on the residuals that indicate that a certain

level of convergence has been achieved. If the residuals for all problem

variables fall below the convergence criteria but are still in decline, the

solution is still changing to a greater or lesser degree. A better indicator

occurs when the residuals flatten in a traditional residual plot (of residual

value vs. iteration). This point, sometimes referred to as convergence at

the level of machine accuracy, takes time to reach, however, and may

be beyond your needs. For this reason, alternative tools such as reports

of forces, heat balances, or mass balances can be used instead.

cortex

A utility that manages ANSYS Fluent’s user interface and basic graphical

functions.

data files

Files that contain the values of the flow field in each grid element and

the convergence history (residuals) for that flow field.

dialog boxes

The separate windows that are used like forms to perform input tasks.

Each dialog box is unique and employs various types of input controls

that make up the form.

discretization

The act of replacing the differential equations that govern fluid flow with

a set of algebraic equations that are solved at distinct points.

GUI

The graphical user interface, which consists of the main ANSYS Fluent

application window, dialog boxes, graphics windows, etc.

mesh

GUI

mesh

A collection of points representing the flow field, where the equations

of fluid motion (and temperature, if relevant) are calculated.

models

Numerical algorithms that approximate physical phenomenon (for ex-

ample, turbulence).

node

The distinct points of a mesh (p. ) at which the equations of fluid

motion are solved.

postprocessing

The act of analyzing the numerical results of your CFD simulation using

reports, integrals, and graphical analysis tools such as contour plots, an-

imations, etc.

residuals

The small imbalance that is created during the course of the iterative

solution algorithm. This imbalance in each cell is a small, non-zero value

that, under normal circumstances, decreases as the solution progresses.

skewness

The difference between the shape of the cell and the shape of an equi-

lateral cell of equivalent volume. Highly skewed cells can decrease accur-

acy and destabilize the solution.

solvers

ANSYS Fluent has two distinct solvers, based on numerical precision

(single-precision vs. double-precision). Within each of these categories,

there are solver formulations: pressure based; density based explicit; and

density based implicit.

terminal emulator

See console (p. ).

TUI

The text user interface, which consists of textual commands that can be

entered into the terminal emulator.

Part II: Meshing Mode

The section describes how to use ANSYS Fluent in meshing mode.

Introduction to Meshing Mode in Fluent (p. ) introduces the meshing mode in Fluent and gives an overview

of its capabilities.

Starting Fluent in Meshing Mode (p. ) provides instructions for starting Fluent in meshing mode.

Graphical User Interface (p. ) describes the use of the graphical user interface and explains how to use

the online help system.

Text User Interface (p. ) introduces the text-based user interface.

Reading and Writing Files (p. ) describes the file types that can be read and written (including picture

files) and gives details for importing CAD geometry.

Working With Fluent Guided Workflows (p. ) describes the guided meshing workflows that make it easier

to generate a volume mesh starting from CAD geometries.

CAD Assemblies (p. ) describes additional tools for imported CAD data in Fluent Meshing.

Size Functions and Scoped Sizing (p. ) describes how to control the mesh size distribution on a surface

or within the volume.

Objects and Material Points (p. ) describes the use of objects and material points for identifying the mesh

region.

Object-Based Surface Meshing (p. ) describes the object-based workflow for generating a conformal,

connected surface mesh.

Object-Based Volume Meshing (p. ) describes how to fill the good quality surface mesh with tet, hexcore,

poly, or hybrid volume mesh.

Manipulating the Boundary Mesh (p. ) explains the need for a high-quality boundary mesh and describes

the various options available for creating such meshes.

Wrapping Objects (p. ) describes the option for creating a high-quality boundary mesh starting from bad

surface mesh using the boundary wrapper tool.

Creating a Mesh (p. ) describes the zone-based meshing strategy and the creation of pyramids, non-

conformals, and heat exchanger meshes.

Generating Prisms (p. ) describes the procedure to create inflation layers in your volume mesh. It also

explains how to deal with common problems that can be faced while creating prisms.

Generating Tetrahedral Meshes (p. ) describes the meshing procedures for tetrahedral meshes.

Generating the Hexcore Mesh (p. ) describes the procedure and options for creating Cartesian cells in

the interior of the domain.

Generating Polyhedral Meshes (p. ) describes the procedure and options for creating polyhedral meshes.

Generating Poly-Hexcore Meshes (p. ) describes the procedure and options for creating poly-hexcore

meshes.

Generating the CutCell Mesh (p. ) describes the CutCell meshing procedure and options available for

CutCell meshing.

Improving the Mesh (p. ) describes the options available for improving the quality of a volume mesh.

Examining the Mesh (p. ) describes the methods available for examining the mesh graphically.

Determining Mesh Statistics and Quality (p. ) describes methods for checking the mesh diagnostically.

Appendix A: Importing Boundary and Volume Meshes (p. ) describes filters that you can use to convert

data from various software packages to a form that can be read.

Appendix B: Mesh File Format (p. ) describes the format of the mesh file.

Appendix C: Shortcut Keys (p. ) lists all the hot-keys (shortcut keys) available.

Bibliography (p. ) presents the bibliography for the previous chapters.

Chapter : Introduction to Meshing Mode in Fluent

When in meshing mode, Fluent functions as a robust, unstructured mesh generation program that can

handle meshes of virtually unlimited size and complexity. Meshes may consist of tetrahedral, hexahedral,

polyhedral, prismatic, or pyramidal cells. Unstructured mesh generation techniques couple basic geo-

metric building blocks with extensive geometric data to automate the mesh generation process.

A number of tools are available for checking and repairing the boundary mesh to ensure a good starting

point for generating the volume mesh. The volume mesh can be generated from the boundary mesh

using one of the approaches described.

The user interface is written in the Scheme language, which is a dialect of LISP. Most features are ac-

cessible through the graphical interface or the interactive menu interface. The advanced user can cus-

tomize and enhance the interface by adding or changing the Scheme functions.

.. Meshing Approach

There are two principal approaches to creating meshes in ANSYS Fluent Meshing:

Generate a tetrahedral, hexcore, or hybrid volume mesh from an existing boundary mesh. In this case, you

can import a boundary mesh from ANSYS Meshing or a third-party mesh generation package.You can import

boundary meshes created in CAD/CAE packages by using the appropriate menu item in the File → Import

submenu (or the associated text commands), or you can convert them using the appropriate stand-alone

grid filter.

Generate a tetrahedral, hexcore, or hybrid volume mesh based on meshing objects from a faceted geometry

(from CAD or the .tgf format from ANSYS Meshing). In this case, you need to create a conformally connected

surface mesh using the object wrapping and sewing operations before generating the volume mesh.You

can alternatively use the CutCell mesher to directly create a hex-dominant volume mesh for the geometry

(imported from CAD or the .tgf format from ANSYS Meshing) based on meshing objects.

When the mesh generation is complete, you can transfer the mesh to solution mode using the Mode

toolbar or the command switch-to-solution-mode. The remaining operations—such as setting

boundary conditions, defining fluid properties, executing the solution, and viewing and postprocessing

the results—are performed in solution mode (see the User’s Guide (p. ) for details).

.. Meshing Mode Capabilities

When in meshing mode, Fluent:

Functions as a robust, unstructured volume mesh generator

Generates volume meshes that can be transferred to solution mode in Fluent

Uses the Delaunay triangulation method for tetrahedra

Uses the advancing layer method for prisms

Generates hexcore mesh

Has a robust surface wrapper tool

Includes size functions that can produce ideal size distributions for many CFD calculations

Can directly create a hex-dominant mesh on faceted geometry (using the CutCell mesher)

Can export polyhedral cells

Has tools for checking, repairing, and improving boundary mesh to ensure a good starting point for the

volume mesh

Can manipulate face/cell zones

Is flexible—it allows the most appropriate cell type to be used to generate the volume mesh:

– Tet meshes are suitable for complex geometries.

– Hexcore meshes can combine the flexibility of tet, hex, and prism meshes with a smaller cell count and

higher hex-to-tet ratio.

– CutCell (hex-dominant) meshes can be directly created from faceted geometry and can also be combined

with prism layers.

Has hybrid meshes:

– Prism layers near walls allow proper boundary layer resolution.

– Allows flow alignments with mesh lines.

– Generates smaller volume mesh with highly stretched prismatic elements.

Has non-conformal meshes:

– Suitable for studies involving selective replacement of parts.

– Meshes generated separately can be glued together.

Introduction to Meshing Mode in Fluent

Chapter : Starting Fluent in Meshing Mode

Starting Fluent in meshing mode is accomplished by enabling the Meshing Mode checkbox under

Options in the Fluent Launcher, or by adding the directive -meshing when using the command line

interface.

See Starting and Executing ANSYS Fluent (p. ) in the Fluent Getting Started Guide for full details on

setting dimension and other options for starting in meshing mode.

The .tgrid File

When starting up in meshing mode, Fluent looks in your home directory for an optional file called

.tgrid. This file is then loaded using the Scheme function load. You can use the .tgrid file to

customize the operation of the code in meshing mode.

For example, the Scheme function ti-menu-load-string is used to include text commands in the

.tgrid file. If the .tgrid file contains (ti-menu-load-string "file read-case test.cas"),

then the case file test.cas will be read in. For more details about the function ti-menu-load-

string, see Text Menu Input from Character Strings in the Fluent Text Command List.

Important

Important

Another optional file, .fluent, if present, is also loaded at start up. This file may contain

Scheme functions that customize the operation of the code in solution mode. When both

the .tgrid and .fluent files are present, the .fluent file will be loaded first, followed

by the .tgrid file, when the meshing mode is launched. Hence, the functions in the .tgrid

file will take precedence over those in the .fluent file for the meshing mode.

The .fluent file is not loaded again automatically when switching to solution mode from

meshing mode. You will need to load the file separately using the Scheme load function,

if needed.

.. Starting the Dual Process Build

The dual process build allows you to run Cortex on your local machine (host) and Fluent on a remote

machine. The advantage of using the dual process build is faster response to graphics actions (such as

zoom-in, zoom-out, opening a dialog box, and so on) when you use Fluent remotely. If the network

connectivity is slow, then graphics actions may appear slow and jerky. By controlling the graphics actions

locally, the slow response of the graphics actions can be avoided. For example, if you are handling a

big mesh (such as the underhood mesh), you can start a dual process build to run Fluent remotely with

only the display set to your local machine.

To start the dual process build of Fluent in meshing mode, do the following:

.

Start Fluent on your local machine using the command fluent -serv -meshing.

The Fluent window will appear with the version prompt in the console.

.

Type listen and press Enter.

.

.

You will be prompted for a timeout (the period of time to wait for a connection from remote Fluent).

The default value is  seconds. You can also specify the timeout value based on your requirement.

Utilize this time to log into the remote machine and to start Fluent.

.

Press Enter again.

A message will prompt you to start Fluent on the remote machine with the following arguments:

cx host:p1:p2

where,

host is the name of the host (local) machine on which Cortex is running.

p1 and p2 are the two integers indicating the connecting port numbers that are used to commu-

nicate information between Cortex on the host machine and Fluent on the remote machine.

.

Login to the remote machine and set the display to the host machine.

.

Start Fluent from the remote machine using the following command: fluent 3d -cx host:p1:p2

The host and port numbers are displayed in the message window.

Note

The user interface commands related to the File menu (such as reading files, importing files)

and other Select File dialog boxes do not work for the dual process build. You need to use

the TUI commands instead (for example, /file/read-mesh).

Important

The host cannot be detached and reattached; once the connection is broken the data is lost.You

need to save the data if the machine needs to be shut down in between.

All graphics information will be sent over the network, so initially it could take a long time to

assemble graphical information (especially if the host and remote server are across continents)

but after that the graphics manipulation is fast.

.. Dynamically Spawning Processes Between Fluent Meshing and Fluent

Solution Modes

For parallel simulations started in meshing mode with more than one process, the Fluent session will

be started by using the number of processes requested for meshing. When switching to solution mode,

Fluent will automatically spawn the remaining parallel node processes needed to achieve the requested

number of total solution processes. Even though automatic spawning is used by default at start up for

runs using more than one process, you can always change the number of additional processes to be

Starting Fluent in Meshing Mode

spawned before switching to solution mode using the /parallel/spawn-solver-process text

user interface (TUI) command.

This text command prompts you for:

Total number of desired processes (must be greater than or equal to the number of meshing processes).

Fluent will spawn additional processes as necessary.

(Linux and mixed Windows / Linux) Interconnect type to be used for the distributed parallel simulation.You

can choose from infiniband, ethernet, shared memory, or you can retain the default value.

Machine list or host file. If you decide to run in parallel using more than one machine, then you should

provide the machine list or host file, otherwise, you can skip this option by pressing Enter.

(Linux and mixed Windows / Linux) Option to use ssh for distributed simulations, otherwise, you can skip

this option by pressing Enter to retain the default option.

Important

Note the following:

Dynamic process spawning is not supported on Cray systems.You can keep the same

Important

number of cores for meshing mode as for solver mode, however, you should continue the

solver iterations using another separate solver session.

Dynamic process spawning is only supported with the following MPIs:

– default

– ibmmpi

While running under the Fluent–supported load managers (for example, SGE/LSF/PBS

Pro), the total number of required parallel node processes must be requested at the

start of Fluent session, and Fluent will initially start with the specified number of

processes for meshing mode and will automatically spawn the remaining node pro-

cesses while switching to solution mode.

Using a single machine host file with different numbers of meshing and solver cores at the

start of an ANSYS Fluent session may result in an unintended host allocation. Instead, you

should specify a machine host file only for the initial (meshing) mode.Then before switching

from the meshing to the solution mode, you should use the parallel/spawn-solver-

processes text command to request additional cores and specify a separate machine host

file for the additional cores.

Dynamically Spawning Processes Between Fluent Meshing and Fluent Solution Modes

Chapter : Graphical User Interface

The graphical user interface (GUI) components are illustrated in Figure . : The User Interface Compon-

ents (p. ). The interface will change depending on whether you are in meshing mode (as described

in this guide) or solution mode (as described in the Fluent User's Guide (p. )). For details on switching

between the meshing and solution mode, see Solution (p. ).

Figure . : The User Interface Components

Object-based meshing is a context-driven, visual workflow, accessible using the major interface com-

ponents. A complete description of the components is found in the User Interface Components (p. )

section.

Menu bar commands are appropriate for zone-based meshing or advanced display and report options.

Full descriptions of the menu commands are in their related chapters in this manual.

Some of the user interface elements can be moved or tabbed together to suit your preferences. You

can also modify attributes of the interface (including colors and text fonts) to better match your platform

environment. These are described in Customizing the User Interface (p. ).

The help button (

) accesses a drop down list for quick access to the integrated help system, including

the Fluent User's Guide. The Fluent integrated help system is described in detail in Using the Help Sys-

tem (p. ).

.. User Interface Components

The components are described in detail in the subsequent sections.

...The Ribbon

...The Workflow Tab

...The Outline View Tab

...The Graphics Window

... Quick Search

...The Console

...The Toolbars

... ACT Start Page

In Mesh Generation mode, the ribbon contains options to help with managing the graphical display,

selecting objects or zones, and patching options.

Note

When working with CAD Assemblies, certain meshing ribbon tools are disabled.

The hide ribbon button (

) is used to minimize the ribbon, allowing more area for the graphics

window. Click a second time to maximize the ribbon to restore the graphics window area.

Solution

The Switch to Solution option enables you to switch from meshing mode to solution mode.

Solution

It transfers all of the volume mesh data from meshing mode to solution mode in ANSYS Fluent.

You will be asked to confirm the mesh is valid and that you want to switch to solution mode.

Important

Only volume meshes can be transferred to solution mode; surface meshes cannot be

transferred.

Face zones which are not connected to volume mesh (geometry objects or un-

referenced zones in case of mesh object-based workflow) will be transferred as

imported surfaces when the volume mesh is transferred from meshing to solution

mode. Also, any unmeshed face zones connected to volume mesh (mesh object

with some regions filled or unreferenced zones), will be disconnected and

transferred as imported surfaces in solution mode.

You should check that the mesh quality is adequate before transferring the mesh data

to solution mode. See Checking the Mesh (p. ) and Checking the Mesh Quality (p. )

Graphical User Interface

for details.When you are satisfied with the quality of the generated mesh, you can

proceed to solution mode.

Hanging-node meshes are converted to polyhedra during mesh transfer.

Important

In object-based workflows, merging cell zones requires that they be in the same

volumetric region.

To merge cell zones that cannot be in the same volumetric region because they

are not contiguous, you will need to first delete the object(s) only, and then use

the Manage Cell Zones dialog box.

Note

The command switch-to-solution-mode corresponds to the Switch to Solution

button.

You cannot switch back from solution mode to meshing mode after the mesh data has

been transferred.

Note

button.

However, if no file has been read in solution mode, you can use the command

switch-to-meshing-mode to switch to meshing mode to generate a mesh

to be transferred, if you desire.

The meshing and solution modes in Fluent have different options available for some

user configuration settings.Thus, these configuration settings may be changed when

switching from meshing to solution mode and may not be the same when returning

to one mode after using the other.

Bounds

Use the Bounds group to limit the display region based on proximity to a selected entity in your

model.

Selection is used to specify the entity on which the Bounds are centered.

You can set a selection filter and then click to select the entity in the graphics window.

Set symmetrical upper and lower distance limits in the +/- Delta text box.

Limit the bounds directionally with the X-, Y-, and Z-Range checkboxes.

Use Set Ranges to apply the display limits. Reset disables the bounds display.You will have to

redraw to see the effect.

If Cutplanes is checked, the display region is linked to the Bounds tab in the Display Grid dialog

box.You may insert up to six cutplanes (two in each of the x-, y-, and z-direction) and asymmetrically

control their location. See Generating the Mesh Display Using the Display Grid Dialog Box (p. ).

User Interface Components

Clipping Planes

Crops the display region along the coordinate system axes when Insert Clipping Planes is enabled.

The slider allows interactive position of the clipping plane.

Use the Flip checkbox to reverse the direction of the clipping plane.

Use the Show Cut Edges option to display the cut edges of the model exposed by the clipping

plane. This option is disabled by default.

Use the Draw Cell Layer checkbox to visualize a layer of cells of the volume mesh on the

clipping plane. This option is disabled by default. Once the Draw Cell Layer option is enabled,

use the Freeze Cell Layer checkbox to keep the displayed layer of cells in place while you

perform additional mesh display operations.

To draw a layer of cells on the clipping plane for specific cell zones, select the cell zone(s)

under Mesh Objects in the Tree and use the Draw Cell Layer option in the context menu.

Selection Helper

Use the Selection Helper group to assist in selecting face zones, edge zones, objects, object face

zones, or object edge zones by a Name Pattern and Geometry Recovery level. Select the type of

zone or object using the Filter drop down list, then use the Name Pattern field to refine your selec-

tion.When selecting Face Zones in the Filter list, the Geometry Recovery option is available to

further refine your selection.

The Advanced... button opens the Zone Selection Helper dialog box. Use this dialog box to

expand the zone selection criteria to include the number of entities present in them, or using

the minimum or maximum face zone area.

The Selection Helper options and the Zone Selection Helper dialog box may be used with

all dialog boxes that contain zone or object lists (for example, Cell Zones and Boundary

Zones dialog boxes).

Mouse Probe Function

Use the Mouse Probe Function group to set the behavior of the mouse probe button.

Select

Select

enables the selection of a single entity based on the filter selected and also adds the selected

entity to a list that can be used in most dialog boxes.

Box

enables the selection of a group of entities within a box.To define the selection box, click the

mouse probe button at one corner of the region to be selected, drag the mouse to the opposite

corner, and release the mouse probe button.

Polygon

enables the selection of a group of entities within a polygonal region.To define the selection

polygon, click the mouse probe button at one vertex of the polygonal region to be selected, and

use the left mouse button to successively select each of the remaining vertices.

Click the mouse probe button again (anywhere in the graphics window) to complete the

polygon definition.

Select Visible Entities

enables selection of only visible entities (nodes, faces, zones, objects) when the mouse probe

function is set to Box or Polygon.The selection includes only entities visible to the eye, and not

those hidden behind other entities in the display.This option is disabled by default.When enabled,

ensure that the model is zoomed to an appropriate level for correct selection.

Note

If the mesh is not connected, all entities (nodes, faces, zones, objects) will be selected

irrespective of whether they are visible or not.

This visual selection behavior works only on local displays and may generate

warning messages when attempting selection on a remote system.

Note

For additional mouse probe function options, see Controlling the Mouse Probe

Function (p. )

Display

Note

Display

contains options to control the display in the graphics window.

All Faces

enable or disable the display of all faces in the visible zones or objects, colored by their zone

type.

Free Faces

enable or disable the display and highlighting of free faces on the visible zones or objects. A free

face is one having at least one edge not shared with a neighboring face.

Multi Faces

enable or disable the display of multi-connected faces on the visible zones or objects, along with

their nodes. A multi-connected face is a boundary face that shares an edge with more than one

other face, while a multi-connected node is a node that is on a multi-connected edge (that is,

an edge that is shared by more than two boundary faces).

Face Edges

enable or disable the display of face edges in the visible zones or objects.This option works in

conjunction with the All Faces option.

Title

enable or disable the display of the caption block area below the graphic containing date, product,

and contents of the display.

Help Text

enable or disable the display of help text for tool buttons or hot-keys. Detailed help is displayed

whenever a command is selected by clicking a button (or pressing a hotkey on the keyboard),

and remains visible until the command is complete or another command selected.

Highlight

enable or disable the highlighting of objects, face zone labels, volumetric regions, or cell zones

selected in the tree.

Edge Zones

enable or disable the display of edge zones comprising the objects drawn in the graphics window.

Transparency

Edge Zones

toggle the transparency of the selected objects/zones depending on the mode of selection set.

If no object/zone is selected then the entire geometry is made transparent so that internal ob-

jects/zones are visible.

Explode

toggle between a normal view and an exploded view of the objects in the geometry.

Edge Zone Selection Mode

enable or disable the edge zone selection mode.This restricts selection to edge zones entities

only.

Edges

show or hide edges on selected zones and objects independent of the mode of selection. If no

object/zone is selected, then the edges on the displayed zones/objects are shown/hidden.

Examine

contains options for obtaining additional information about the selected entities.

Centroid

prints the coordinates of the centroid of the selected face to the console.

This also works for edges and nodes.

Distance

calculates and displays the distance between two selected locations or nodes.

Entity Information

prints detailed information about the selected entities in the message window. For more details,

see Entity Information (p. ).

In addition, if a selected zone or object has been set as a target, this will toggle the

identifying color.

Patch Options

contains additional options applicable to the patching tools.

Remesh

enables automatic remeshing of the patched area.

Separate

enables you to create a separate face zone/object for the new faces created. Additional options

for object/zone granularity and type are available in the Patch Options dialog box (see Using

the Patch Options Dialog Box (p. ) for details).

The Remesh and Separate options are enabled by default.

Use the Workflow tab to access guided workflow templates that can be used to streamline the use

of Fluent in meshing mode. Common tasks and property settings are available to walk you through

the process of generating a volume mesh for use in the Fluent solver. For instance, the Watertight

Geometry guided workflow can be used to quickly generate a volume mesh from an imported watertight

CAD geometry. You can also create your own workflow using the available tasks (such as, adding local

sizing controls, creating a surface mesh, capping inlets and outlets, creating regions, and so on). See

Working With Fluent Guided Workflows (p. ) for more information.

Figure . : The Watertight Geometry Workflow

In Mesh Generation mode, you use the Outline View tree for object-focused management of the

meshing workflow and display. Branches can be expanded and collapsed as required. At each level,

right-click and select from context-sensitive menus to manage the mesh generation process.

Figure . : The Outline View Tree

Figure . : Model Level Menu

At the top of the tree, right-click Model to access controls not specific to any entity. For example, you

can access dialog boxes to create new construction geometry or objects; set mesh size parameters;

and manage material points, periodicity, and user-defined groups. You can also prepare the mesh for

solving in solution mode.

Figure . : CAD Assemblies Tree

The CAD Assemblies tree is created when the Create CAD Assemblies option is selected for CAD

import. It represents the CAD tree as it is presented in the CAD package in which it was created. The

CAD entities in the tree are categorized as components and bodies. Components represent an assembly,

sub-assembly, or part in the original CAD package, while bodies are the basic entities which include

CAD zones. You can also set up labels for the CAD zones, if required.

Figure . : CAD Assemblies Menu

Right-click CAD Assemblies to draw or delete all imported assemblies, and obtain the referenced

FMDB file locations. The Tree sub-menu contains options that control the appearance of the CAD As-

semblies tree. These options can be used to select or deselect the CAD objects and zones in the tree,

expand or collapse the tree branches, and also delete suppressed or locked CAD objects.

Figure . : CAD Component/Body Level Menu

The tree menus at CAD component and body levels contain display options and options for updating

the CAD entities, creating and manipulating geometry/mesh objects, setting the state and modifying

the CAD entities, and tree selection options.

Figure . : CAD Label Level Menu

The CAD label menu contains options for deleting and renaming the labels.

For a full description of the CAD Assemblies tree menus, see CAD Assemblies (p. ).

Geometry and Mesh Objects

When reading a mesh file, the tree is populated with Geometry Objects and Mesh Objects, if already

defined. Importing a mesh from other formats will result in the edge zones, boundary face zones, and

cell zones available in the Unreferenced branch. These zones are not included in any object.

Geometry objects are created when CAD files are imported using the CAD Faceting option. The geo-

metry objects may be non-conformal. Mesh objects are created when CAD files are imported using

the CFD Surface Mesh option. The mesh objects are conformal. See Importing CAD Files (p. ) for

details on the CAD import options.

You can also create geometry/mesh objects from the CAD entities in the CAD Assemblies tree. CAD

entities are locked when corresponding geometry or mesh objects are created. See Creating and

Modifying Geometry/Mesh Objects (p. ) for details.

Figure . : Global Object Level Menu

You use the Geometry Objects or Mesh Objects context-sensitive menu to perform actions on all

objects in your model. At the global object level, right-click (Geometry Objects or Mesh Objects) to

draw or select all the objects.

If the objects are associated with CAD entities, you can also update all or detach all objects.

Figure . : Individual Object Level Menu

Right-clicking on an individual Object (Geometry or Mesh) name in the Outline View opens a context-

sensitive menu to access object level refinement and control tasks. You can also select objects graph-

ically, but the menus are available only when selecting in the Outline View.

Figure . : Face Zone Labels Level Menu

For geometry objects, Face Zone Labels are groups of face zones comprising the object. For mesh

objects, these are original CAD zones or bodies, or face zones comprising the mesh object. If the mesh

object is created by merging multiple mesh objects, the face zone labels represent the objects that

were merged. They provide the link to the original geometry. Under Mesh Objects, Face Zone Labels

form boundaries enclosing the Volumetric Regions--separate, closed, water-tight volumes. Cell Zones

are regions of volume mesh.

The context-sensitive menu for Face Zone Labels contains options for drawing and selecting all labels,

creating new labels, and obtaining an overall summary or detailed information about the face zone

labels. For geometry objects, there are additional options to remove labels from zones and options

for displaying and selecting unlabeled zones. For mesh objects, the Join/Intersect... option contains

options for creating a conformal surface mesh.

Figure . : Individual Label Menu

Right-clicking on a Zone Label name under geometry/mesh objects allows for zone level display and

selection options, and meshing tasks.

Figure . : Unreferenced Zones Menu

The Unreferenced menu includes the common Draw and List Selection menus as well as options to

manage the unreferenced zones.

For a full description of object based meshing using the tree and context menus, refer to Surface Mesh

Processes (p. ).

Note

Any dialog box opened via right-clicking in the Outline View becomes modal. That is, to

preserve the active selection, the action must be completed or the dialog box closed before

the tree selection can be changed.

The graphics window displays the current state of your model according to your selected Rendering,

Color Scheme and Display options. See Controlling Display Options (p. ) for details.

) is used to expand the area for the graphics window by minimizing the

ribbon. Click a second time to maximize the ribbon to restore the graphics window area.

The axis triad indicates the orientation of the model and also provides options for manipulating the

orientation in the graphics window.

To change the orientation of the model using the triad, you can:

Click an axis/semi-sphere to orient the model in the positive/negative direction.

Right-click an axis/semi-sphere to orient the model in the negative/positive direction.

Click the cyan iso-ball to set the isometric view.

Click the white rotational arrows to perform in-plane clockwise or counterclockwise  degree rotations.

Left-click and hold--in the vicinity of the triad--and use the mouse to perform free rotations in any direction.

Release the left mouse button to stop rotating.

You can choose how the mouse buttons interact with the graphics display using the Mouse Buttons

dialog box. See Controlling the Mouse Buttons (p. ).

The search bar (upper right of the Fluent window) allows you to quickly locate the commands or

controls that you are looking for. Clicking the search results is equivalent to clicking the same control

in the ribbon. Hovering over a search result highlights the location of the control in the ribbon. Clicking

a text command search result automatically enters the text of the command, but it does not execute

the command; you still have to press Enter in the console to execute the text command.

The console is usually located below the Graphics Window, as shown in Figure . : The User Interface

Components (p. ). It is used to provide a text based interface to Fluent meshing.

The console will display messages relating to meshing or solution procedures. All console information

is saved to memory, so you can review it at anytime by using the scroll bar on the right side of the

console.The console visually indicates whether the text is an error message (red), user input (blue),

or program generated output (black).

The console behaves like an "xterm" or other Linux command shell tool, or to the MS-DOS Command

Prompt window. It enables you to interact with the TUI menu. For more information on the TUI, see

Text User Interface in the Fluent Text Command List.

You may interrupt the program by issuing a "break" command (press Ctrl+C) while data is being pro-

cessed.You cannot cancel an operation after it is complete and the program has started drawing in

the graphics window.

You may perform text copy and paste operations between the console and other X Window (or Win-

dows) applications that support copy and paste.

Note

On a Linux system, follow the steps below to copy text to the clipboard:

. Drag the pointer across the text to be copied.

. Move the pointer to the target window.

. Press the middle mouse button to “paste” the text.

The Auto-scroll check box enables automatic scrolling of the console when new content is printed.

When the Auto-scroll is disabled, the cursor stays at the last selected position. Messages will continue

to be appended in the console, but the cursor will not automatically scroll to the bottom until the

Auto-scroll is enabled.

The user interface includes several toolbars to provide shortcuts to performing common tasks. You

can enable or disable the visibility of the toolbars that appear in the graphical user interface. You can

dock the toolbars around the graphics window or position them "floating" at any convenient location

in the user interface.

The Standard Toolbar contains options to control the layout and to find additional resources.

Click the ANSYS logo to open the ANSYS home page in your default browser.

Use the options in the Arrange the workspace (

) menu to control the application window layout.You

can also enable or disable the visibility of each interface component in this menu.

The most recent arrangement of the user interface components will be saved to a .cxlayout file

in your home folder. The layout will be restored the next time ANSYS Fluent is opened.

Note

Do not use multiple graphics windows in meshing mode.

Help (

) contains options for accessing the User Documentation and obtaining license usage and product

version information. See Using the Help System (p. ) for details.

On each side of the graphics window are context-sensitive toolbars for quick access to commonly used

operations. Right-click any toolbar to access the Toolbar Options to set the visibility of the respective

toolbars.

.... Pointer Tools

You can quickly change the role of the left mouse button using the options in the Pointer Tools

toolbar. See Controlling the Mouse Buttons (p. ) for a description of the options.

Rotate View

assigns the mouse-rotate function to the left mouse button.

Pan

assigns the mouse-dolly function to the left mouse button.

Zoom In/Out

assigns the mouse-roll-zoom function to the left mouse button.

Zoom to Area

assigns the mouse-zoom function to the left mouse button.

....View Tools

You can quickly change the model display using the View Tools toolbar.

Fit to Window

adjusts the overall size of your model to take maximum advantage of the graphics

window’s width and height.

Last View

restores the display to the previous view.

Set view

contains a drop-down of views, allowing you to display the model in isometric or one of

six orthographic views.

You can also click on the display axes triad in the graphics window to change to one of the

standard views. Use the right mouse button to reverse the orthographic view.

Save Picture

captures an image of the active graphics window. For more information, see Saving

Picture Files (p. ).

.... Projection

Use the Projection toolbar to choose to display a perspective view of the graphics (default) or an

orthographic view.

When the orthographic view is enabled, the ruler is enabled in the graphics window.

.... Display Options

This toolbar is applicable only in solution mode. See Mesh Display Configuration (p. ) for details.

.... Additional Display Options

There are additional display options available when working in the graphics window:

Ruler

turns the ruler on and off (and switches the view to orthographic).

Grid Display

opens the Display Grid dialog where you can select options for displaying the mesh.

See Generating the Mesh Display Using the Display Grid Dialog Box (p. ) for more information.

Front Faces Transparent

makes the front faces of the displayed object transparent, allowing you to

see inside.

Axes Visibility

turns the axes display on and off.

Titles Visibility

turns the titles on and off.

.... Filter Toolbar

Use the Filter toolbar to set the entity type that the mouse probe filter will recognize. See Controlling

the Mouse Probe Function (p. ).

The selection filters available in the toolbar are Position, Node, Edge, Zone, and Object. You can

also set the mouse probe to Draw Sizes and examine the mesh size at the probe point.

The toolbar also contains options for selecting visible entities based on the filter set, deselecting the

last entity, and clearing all selections.

.... CAD Tools

Use the CAD Toolbar to access tools for manipulating CAD entities and creating/managing labels

and geometry/mesh objects associated with the CAD entities. This toolbar is available only when the

CAD entities are displayed in the graphics window.

See CAD Assemblies (p. ) for details.

....Tools

Use the Tools toolbar to access options for constructing geometry primitives or loop selection tools.

....Tools

You can also use the Isolate tools to isolate selected zones/objects in the display or limit the display

to zones/objects based on area/curvature of the selected zones/objects.

.... Context Toolbar

Use the Context toolbar to see context-sensitive options based on the entities selected. When entities

are selected with the mouse probe, this toolbar changes to represent the tasks and processes applicable

to the selected entities, as a subset of all tasks and processes used to generate a mesh.

An example is shown below. Descriptions of available tools are compiled in Shortcut Key Actions (p. ).

The ACT Start Page is available when ACT functionality is enabled in Fluent. To enable ACT function-

ality, use one of these options:

Enable Load ACT in the Fluent Launcher.

Select ACT from the Arrange the workspace (

) menu.

Use the command: /file/load-act-tool.

The ACT Start Page provides an access point for ANSYS ACT functionality in Fluent. From this page,

you can access tools that can be used in the development and execution of extensions. For more in-

formation, see ACT Tools in the ANSYS ACT Developer's Guide.

For information on creating target product wizards for Fluent, see the ACT Customization Guide for

Fluent.

.. Customizing the User Interface

You may want to customize the graphical user interface by changing the way that the various elements

are arranged. This can be achieved by "dragging" elements and "dropping" them at a new location. For

example, the graphics window can be tabbed on top of the console, or the console can be moved below

the tree. In meshing mode, you can move the console and the toolbars.

To restore items that you intentionally or unintentionally closed, right-click the top toolbar to restore

those items. You can also click

to select one of the predefined layouts and restore missing items.

You may also want to customize the graphical user interface by changing attributes such as text color,

background color, and text fonts. The program will try to provide default text fonts that are satisfactory

for your platform's display size, but in some cases customization may be necessary if the default text

fonts make the GUI too small or too large on your display, or if the default colors are undesirable.

The GUI in Fluent is based on the Qt Toolkit. If you are unfamiliar with the Qt Toolkit, refer to any

documentation you may have that describes how to use the Qt Toolkit or application. The graphical

attributes can be modified in a Qt stylesheet file named cxdisplay.qss and placed in your home

.. Setting User Preferences/Options

You can specify global settings that are applied whenever you are operating in ANSYS Fluent. These

settings are case-independent and are controlled using the Preferences dialog box.

To review and modify your preferences, open the Preferences dialog box by selecting Preferences...

from the File menu.

File → Preferences...

Setting User Preferences/Options

Figure . : Preferences Dialog Box

Note

Some settings, such as ruler visibility and mouse-button controls, can also be controlled locally

within a Fluent session (that is, outside of the Preferences dialog box). Settings that deviate from

the global settings specified in the Preferences dialog box will not be retained beyond the current

session.

.. Using the Help System

Fluent includes an integrated help system that provides an easy access to the documentation. Using

the graphical user interface, you can access the entire User's Guide and other documentation. The User's

Guide and other manuals are displayed in the ANSYS Help, which enables you to use the hypertext

links and the browser's search and navigation tools to find the information you need.

There are many ways to access the information contained in the online help:

You can get reference information from the main window or any dialog box by clicking Help.

You can request context-sensitive help for a particular menu item or dialog box by selecting Help → Context-

Sensitive Help.

With the resulting question-mark cursor, select an item from a pull-down menu to open the ANSYS

Help at the selected item.

You can go to the contents page for the Meshing section of the User's Guide and use the hypertext links

there to find the information you are looking for. Select Help → User's Guide Contents.

... Help for Text Interface Commands

To find information about text interface commands, you can either go to the Meshing section of the

Fluent Text Command List in the ANSYS Help, or use the text interface help system described in Text

User Interface in the Fluent Text Command List.

... Obtaining a Listing of Other License Users

If you are running with an existing Fluent license (FluentLM), you can obtain a listing of current Fluent

users in the console by selecting Help → License Usage.

If your installation of Fluent is managed by the ANSYS License Manager (ANSLIC_ADMIN), you will see

a message that will indicate that licensing is managed by ANSLIC_ADMIN. For additional information

on licensing information, refer to the Installation and Licensing Documentation in the ANSYS Help.

This information can be found by doing the following in the help viewer:

. Scroll down to the Installation and Licensing Documentation item in the left pane of the viewer.

. Expand this document by clicking on the icon to the left of the document title.

. Use the hyperlinks in the main viewer window to find the desired information, or, expand the items

in the left pane of the viewer and scroll to the topic of interest.

Using the Help System

Chapter :Text User Interface

The text user interface (TUI) in Fluent, also referred to as The Console (p. ), is written in a dialect of

Lisp called Scheme. Users familiar with Scheme will be able to use the interpretive capabilities of the

interface to create customized commands. The text-based menu system provides a hierarchical interface

to the underlying procedural interface of the program.

You can easily manipulate its operation with standard text-based tools—input can be saved in files,

modified using text editors, and read back in to be executed.

The text menu system is tightly integrated with the Scheme extension language, so it can easily be

programmed to provide sophisticated control and customized functionality.

A more complete description of the text-based interface, including a full list of commands is available

in Fluent Text Command List.

Chapter : Reading and Writing Files

During a Fluent session, you may need to:

Read mesh, case, CAD, journal, Scheme, domain, and size-field files.

Write mesh, case, journal, transcript, and domain files.

Save pictures of graphics windows.

These files and operations are described in the following sections.

.. Shortcuts for Reading and Writing Files

.. Mesh Files

.. Case Files

.. Reading and Writing Size-Field Files

.. Reading Scheme Source Files

.. Creating and Reading Journal Files

.. Creating Transcript Files

.. Reading and Writing Domain Files

.. Importing Files

.. Saving Picture Files

The following features make reading and writing files convenient:

... Binary Files

... Reading and Writing Compressed Files

...Tilde Expansion (LINUX Systems Only)

... Disabling the Overwrite Confirmation Prompt

When you write a mesh, case, or size-field file, a binary file is saved by default. Binary files take up less

memory than text files and can be read and written more quickly by Fluent.

To save a text file, disable the Write Binary Files option in the Select File dialog box when you are

writing the file.

Fluent enables you to read and write compressed files. Use the Select File dialog box to read or write

the files that have been compressed using compress or gzip.

.... Reading Compressed Files

....Writing Compressed Files

If you select a compressed file with a .z extension, Fluent will automatically invoke zcat to import

the file. If you select a compressed file with a .gz extension, Fluent will invoke gunzip to import

the file. For example, if you select a file named flow.msh.gz, the following message will be reported,

indicating that the result of the gunzip is imported into Fluent via an operating system pipe.

Reading "\" | gunzip -c \"Z:\flow.msh.gz\"\""...

When reading a compressed file using the text interface, you only need to enter the file name. Fluent

first looks for a file to open using just the input name. If it cannot find a file with that name, it attempts

to locate files with default suffixes and extensions appended to the name. For example, if you enter

the name file-name, it traverses the following list until it finds an existing file to open:

file-name

file-name.gz

file-name.z

file-name.suffix

file-name.suffix.gz

file-name.suffix.z

where suffix is a common extension to the file, such as .cas or .msh. Fluent reports an error if

it fails to find an existing file with one of these names.

Note

For Windows systems, only files that were compressed with gzip (that is, files with a .gz

extension) can be read. Files that were compressed using compress cannot be read into

Fluent on a Windows machine.

You can use the Select File dialog box to write a compressed file by appending a .z or .gz extension

onto the file name. For example, if you are prompted for a file name and you enter a file name with

a .gz extension, a compressed file will be written. For example, if you enter flow.gz as the name

for a mesh file, Fluent reports the following message:

Writing "| gzip -cfv > Z:\flow.msh.gz"...

Reading and Writing Files

The status message indicates that the mesh file information is being piped into the gzip command,

and that the output of the compression command is being redirected to the file with the specified

name. In this particular example, the .msh extension was added automatically.

Note

For Windows systems, compression can be performed only with gzip. That is, you can

write a compressed file by appending .gz to the name, but appending .z does not

compress the file.

On LINUX systems, if you specify ~/ as the first two characters of a file name, the ~ is expanded as

your home directory. Similarly, you can start a file name with ~username/, and the ~username is

expanded to the home directory of “username”. If you specify ~/file as the mesh file to be written,

Fluent saves the file file.msh in your home directory. You can specify a subdirectory of your home

directory as well: if you enter ~/examples/file.msh, Fluent will save the file file.msh in the

examples subdirectory.

By default, if you ask ANSYS Fluent to write a file with the same name as an existing file in that folder,

it will ask you to confirm that it is “OK to overwrite” the existing file. If you do not want ANSYS Fluent

to ask you for confirmation before it overwrites existing files, you can enter the file/confirm-

overwrite? text command and answer no.

Mesh files are created using the mesh generators (ANSYS Meshing, the meshing mode in Fluent, GAMBIT,

GeoMesh, and PreBFC), or by several third-party CAD packages. From the point of view of Fluent, a

mesh file is a subset of a case file (described in Case Files (p. )). The mesh file includes a list of the

node coordinates, connectivity information that tells how the nodes are connected to one another to

form faces and cells, and the zone types and numbers of all the faces (for example, wall-, pressure-

inlet-, symmetry-). The mesh file does not contain any information on boundary conditions, flow

parameters. For information about the format of the CAD package files, see Appendix A: Importing

Boundary and Volume Meshes (p. ), and for details on the mesh file format for Fluent, see Ap-

pendix B: Mesh File Format (p. ).

Note

You can also use the File → Read → Case... menu item to read a mesh file (described in

Case Files (p. )) because a mesh file is a subset of a case file.

Important

If the mesh information is contained in two or more separate files generated by one of the

CAD packages, you can read them one-by-one by selecting Append File(s) in the Select

Mesh Files

File dialog box. You can also read them together and assemble the complete mesh in the

meshing mode.

By default, Fluent saves the mesh files with the suffix .msh. You need not type the suffix while saving

the mesh file, it will be added automatically.

When Fluent reads a mesh file, it first searches for a file with the exact name you typed. If a file with

that name is not found, it will search for a file with .msh appended to the name.

... Reading Mesh Files

To read a mesh, select File → Read → Mesh... to open the Select File dialog box and select the mesh

file to be read.

You can also use this option to read a Fluent mesh file created with GAMBIT, or to read the mesh

contained in a case file.

Note

Reading a case file as a mesh file will result in loss of boundary condition data as the mesh

file does not contain any information on boundary conditions.

Case files containing polyhedral cells can also be read in the meshing mode of Fluent. You can display

the polyhedral mesh, perform certain mesh manipulation operations, check the mesh quality, and so

on.

Important

You cannot read meshes from solvers that have been adapted using hanging nodes. To

read one of these meshes in the meshing mode in Fluent, coarsen the mesh within the

solver until you have recovered the original unadapted grid.

The /file/read-options command enables you to set the following options for reading mesh

files:

Enforce mesh topology:This option is disabled by default. Enabling this option will orient the face zones

consistently when the mesh file is read. If necessary, the zones being read will be separated, such that each

boundary face zone has at most two cell zones as neighbors, one on either side. Also, internal face zones

are inserted between neighboring cell zones that are connected by interior faces.

Check read data:This option enables additional checks for the validity of the mesh. Enabling this option

will check the mesh topology during file read. In case incorrect mesh topology is encountered, warning

messages will be displayed and the erroneous entities will be deleted. Note that in case of mesh topology

errors, no automatic mesh repair is done, and that parts of the mesh may be non-conformal, contain voids,

or be erroneous in other ways.The purpose of the check-read-data option is to enable access to corrupt

files.This option is disabled by default with the assumption that correct data will be read, and to shorten

file read times.

.... Reading Multiple Mesh Files

If the mesh is contained in two or more separate files, you can read them together in Fluent and as-

semble the complete mesh. For example, if you are creating a hybrid mesh by reading in a triangular

boundary mesh and a volume mesh consisting of hexahedral cells, read both files at the same time

using File → Read → Mesh....

.... Reading 2D Mesh Files in the 3D Version of Fluent

You can read 2D meshes from Fluent into the 3D version of Fluent by using File → Import → Fluent

2D Mesh....

... Reading Boundary Mesh Files

To read a Fluent boundary mesh (contained in a mesh file created with GAMBIT or in a Fluent case

file) into Fluent, select File → Read → Boundary Mesh... to open the Select File dialog box and select

the boundary mesh file to be read.

This option is convenient if you want to reuse the boundary mesh from a file containing a large volume

mesh.

If the boundary mesh is contained in two or more separate files, you can read them in together and

assemble the complete boundary mesh in Fluent.

... Reading Faceted Geometry Files from ANSYS Workbench in Fluent

You can read faceted geometry files (*.tgf) exported from ANSYS Workbench in Fluent. To read the

faceted geometry file, use File → Read → Mesh... or File → Read → Boundary Mesh....

The naming of face zones can be controlled by Named Selections defined in ANSYS Workbench. For

details on exporting faceted geometry from ANSYS Workbench, refer to the ANSYS Workbench Help.

... Appending Mesh Files

You can read multiple mesh files one by one instead of reading all of them at once. This process is

called as appending the mesh files. To append files, read in the first mesh file using the Select File

dialog box. Reopen the dialog box and enable Append File(s) and read the remaining files one by

one.

Note

Append File(s) is not accessible while reading the first mesh file.

You can also append files using the command /file/append-meshes-by-tmerge, which uses

the tmerge utility in ANSYS Fluent. There is no graphical interface equivalent for this text command.

Append Rules:

If zone names and IDs are duplicated, they will be modified and the changes will be reported in the console.

Mesh Files

Domain information will be retained during the file append operation. If domain names are duplicated,

they will be modified and the changes will be reported in the console.

Refinement region information will be retained during the file append operation. If region names are du-

plicated, they will be modified and the changes will be reported in the console.

You can append files comprising only edge zones (without face zones).

Edge-face zone associations will be retained during the file append operation.

Zone-specific prism parameter information will be retained during the file append operation.

...Writing Mesh Files

To write a mesh file in the format that can be read by Fluent, select File → Write → Mesh... to open

the Select File dialog box and specify the name of the mesh file to be written.

See Binary Files (p. ) for information about the file format.

The /file/write-options command enables you to set the enforce mesh topology option

for writing mesh files. This option is disabled by default. Enabling this option will orient the face zones

consistently when the mesh file is written. If necessary, the zones will be separated, such that each

boundary face zone has at most two cell zones as neighbors, one on either side. Also, internal face

zones will be inserted between neighboring cell zones that are connected by interior faces.

Note

You should delete dead zones in the mesh before writing the mesh or case file for Fluent.

...Writing Boundary Mesh Files

Fluent enables you to write a mesh file comprising specific boundary zones. This is useful for large

cases where you may want to mesh different parts of the mesh separately and then merge them to-

gether. This enables you to avoid frequent switching between domains for such cases. You can write

out selected boundaries to a mesh file and then create the volume mesh for the part in a separate

session. You can then read the saved mesh into the previous session using the Append File(s) option

and merge the part with the rest of the mesh.

To write a mesh file comprising selected boundaries, select File → Write → Boundaries... menu item

to invoke the Write Boundaries dialog box and select the boundaries to be written.

Case files contain the mesh, boundary and cell zone conditions, and solution parameters for a problem.

They also contain the information about the user interface and graphics environment. Fluent allows

you to read and write either text or binary files, in compressed or uncompressed formats (For details,

see Binary Files (p. ) and Reading and Writing Compressed Files (p. )). Fluent automatically detects

the file type when reading.

Important

Changing the ID of a thread in the meshing mode may affect the case set up. In such cases,

you will be prompted to confirm that you want to proceed with the ID changing operation.

The commands used for reading case files can also be used to read native-format mesh files (as described

in Mesh Files (p. )) because the mesh information is a subset of the case information. The commands

for reading and writing case files are described in the following sections.

... Reading Case Files

...Writing Case Files

To read a case file, select File → Read → Case... to open the Select File dialog box and select the

case file to be read.

Note

Cell hierarchy in case files adapted in the solution mode will be lost when they are read in

the meshing mode.

on.

on.

To write a case file in the format that can be read by Fluent, select File → Write → Case.

Note

See Binary Files (p. ) for information about the save file format.

If you are writing a hexcore or CutCell mesh, enable the Write As Polyhedra check button in the Select

File dialog box. This enables hex cells that are either part of a hanging-node sub-division or are at the

Case Files

boundary of the hex-tet interface, to be converted to polyhedral cells. Enabling this option permits

the export of these cells instead of non-conformal meshes.

Note

Further manipulation of the mesh is restricted after conversion to polyhedra. Only limited

operations like displaying the polyhedral mesh, certain mesh manipulation operations,

checking the mesh quality are available for polyhedral meshes.

Important

Case files that have been read and re-written in the meshing mode are incompatible with pre-

viously saved data files. Do not read previously saved data files with the case file when such

case files are transferred or read in the solution mode.

If the zone topology changes due to operations performed in the meshing mode, you should

verify the case setup after transferring or reading the case in the solution mode.

....Writing Files Using Hierarchical Data Format (HDF)

When writing case files in parallel, you can optionally use the Hierarchical Data Format (HDF). To write

case files using HDF, you can use the same menu options or TUI commands and simply append .h5

to the file name. Alternatively, select HDF5 Case Files from the Files of type drop-down list in the

Select File dialog box.

HDF files are always binary and make use of built-in compression. Thus, they cannot be viewed in a

text editor. However, third-party tools are available that enable you to open and explore the contents

of files saved in HDF format.

Note

Files written in the HDF format cannot be read in the meshing mode.

Size-field files contain the size function definitions based on the parameters specified.

Select File → Read → Size Field... to read a size-field file. This will invoke the Select File dialog box,

where you can specify the name of the size-field file to be read.

Note

If you read a size-field file after scaling the model, ensure that the size-field file is appropriate

for the scaled model (size-field vertices should match the scaled model).

Select File → Write → Size Field... to write a size-field file. This invokes the Select File dialog box,

where you can specify the name of the size-field file to be written.

A Scheme source file can be loaded in three ways: through the menu system as a scheme file, through

the menu system as a journal file, or through Scheme itself.

For large source files, use the Select File dialog box invoked by selecting the File → Read → Scheme...

menu item or the Scheme load function.

> (load "file.scm")

Shorter files can also be loaded with File → Read → Journal... or the file/read-journal command

in the text interface (or its . or source alias).

> . file.scm

> source file.scm

In this case, each character of the file is echoed to the console as it is read in the same way as if you

were typing the contents of the file.

A journal file contains a sequence of Fluent commands, arranged as they would be typed interactively

into the program or entered through the user interface. The user interface commands are recorded as

Scheme code lines in journal files. You can also create journal files manually with a text editor. If you

want to include comments in your file, put a semicolon (;) at the beginning of each comment line.

The purpose of a journal file is to automate a series of commands instead of entering them repeatedly

on the command line. It can also be used to produce a record of the input to a program session for

later reference, although transcript files are often more useful for this purpose (see Creating Transcript

Files (p. )).

Command input is taken from the specified journal file until its end is reached, at which time control

is returned to the standard input (usually the keyboard). Each line from the journal file is echoed to the

standard output (usually the screen) as it is read and processed.

Important

A journal file by design is a simple record/playback facility. It contains no information about

the state in which it was recorded or the state in which it is being played back.

Be careful not to change the folder while recording a journal file. Also, try to recreate the state in which the

journal was written before you read it into the program.

For example, if the journal file includes an instruction for Fluent to save a new file with a specified

name, check that no file with that name exists in your directory before you read in your journal file.

If a file with that name exists and you read in your journal file, it will prompt for a confirmation to

overwrite the old file when the program reaches the write instruction. Because the journal file contains

no response to the confirmation request, Fluent will not be able to continue following the instructions

of the journal file.

Creating and Reading Journal Files

Other conditions that may affect the program's ability to perform the instructions contained in a journal file

can be created by modifications or manipulations that you make within the program.

For example, if your journal file displays certain surfaces, you must read in the appropriate mesh file

before reading the journal file.

Important

At a given time, only one journal file can be open for recording. But you can read a

journal file at any time. You can also write a journal and a transcript file simultaneously.

You can read multiple journal files in one go.

Select the files in the order you want them read in Fluent in the Select File dialog box.

You can also create a journal file that makes calls to other journal files.

The following is an example of such a nested journal file:

/file/read-journal "E:/Example_journals_example1.jou" ""

/file/read-journal "E:/Example_journals_example2.jou" ""

/file/read-journal "E:/Example_journals_example3.jou" ""

Whenever you start recording a journal file, the text command /file/set-tui-version "XX.X"

is added at the top of the file (where XX.X corresponds to the version of ANSYS Fluent that is record-

ing the journal file). This text command can help journals created in an older version to work properly

when used in a newer version, as it will hide the new text user interface (TUI) prompts and restore

the deleted TUI prompts in that newer version.

If you are writing a journal file in a text editor, it is recommended that you add /file/set-tui-

version "XX.X" at the top of the file.

Note

– The specified version must be within two full releases of the version that is running the

journal.

– To specify version  R3, enter "." for "XX.X".

Whether you choose to type the text command in full or use partial strings, complete commands are recorded

in the journal files.

Important

– Only successfully completed commands are recorded. For example, if you stopped an execution

of a command using Ctrl+C, it will not be recorded in the journal file.

– If a user interface event happens while a text command is in progress, the user interface event

is recorded first.

– All default values are recorded.

To start the journaling process, select File → Write → Start Journal.... Enter a name for the file in the

Select File dialog box. The journal recording begins and the Start Journal menu item becomes Stop

Journal menu item. You can end journal recording by selecting Stop Journal, or by exiting the program.

You can read a journal file into the program using the Select File dialog box invoked by selecting File

→ Read → Journal....

Journal files are always loaded in the main (top-level) text menu, regardless of where you are in the

text menu hierarchy when you invoke the read command.

A transcript file contains a complete record of all standard input to and output from Fluent (usually all

keyboard and user interface input and all screen output).

The user interface commands are recorded as Scheme code lines in transcript files. Fluent creates a

transcript file by recording everything typed as input or entered through the user interface, and

everything printed as output in the text window.

The purpose of a transcript file is to produce a record of the program session for later reference. The

transcript file cannot be read back into the program because they contain messages and other output

transcript files.

Important

At a time, only one transcript file can be open for recording. But you can write a transcript

and a journal file simultaneously. You can also read a journal file while a transcript recording

is in progress.

To start the transcription process, select File → Write → Start Transcript.... Enter a name for the file

in the Select File dialog box. The transcript recording begins and the Start Transcript... menu item

becomes the Stop Transcript menu item. You can end transcript recording by selecting Stop Transcript,

or by exiting the program.

A complete mesh may have multiple domains, each having its lists of nodes, faces, and cell zone IDs.

A domain file is all of the domain information written as a separate file. (A mesh file includes the domain

information as one section in the file.)

By convention, domain file names are composed of a root with the suffix .dom. If you conform to this

convention, you do not have to type the suffix when prompted for a filename; it will be added automat-

ically. When Fluent reads a domain file, it first searches for a file with the exact name you typed. If a

file with that name is not found, it will search for a file with .dom appended to the name. When Fluent

writes a domain file, .dom will be added to the name you type unless the name already ends with

.dom.

To read the domain files into Fluent, select File → Read → Domains... to invoke the Select File dialog

box and specify the name of the domain file to be read.

Reading and Writing Domain Files

If a domain that is being read already exists in the mesh, a warning message is displayed. Fluent verifies

if the zones defining the domains exist in the mesh. If not, it will display a warning message.

To write domain files in Fluent, select File → Write → Domains... to invoke the Select File dialog box

and specify the name of the domain file to be written.

You can import the following file formats using the menu items in the Import submenu, or using the

associated text commands:

ANSYS Prep7/cdb files

CGNS files

FIDAP neutral files

GAMBIT neutral files

HYPERMESH ASCII files

I-deas Universal files

NASTRAN files

PATRAN neutral files

CGNS files

For information about the format of these files and details about importing them (if the import commands

are not available on your computer), see Appendix A: Importing Boundary and Volume Meshes (p. ).

For information about changing the options related to mesh import see Reading and Writing Files in

the Fluent User's Guide (p. ).

Importing Multiple Files

You can also import multiple files using the File → Import menu. Select the file format (for example,

ANSYS prep7/cdb) and the mesh type (surface or volume) to open the Select File dialog box. Select

the appropriate files from the Files selection list and click OK.

Appending Multiple External Files

You can also add files of any external format to an existing mesh. This is known as appending files. To

append external files, read or import the first file. Use the File → Import menu and select the appropriate

file format (for example, ANSYS prep7/cdb) and the mesh type (surface or volume). Enable Append

File(s) in the Select File dialog box and import the necessary files.

... Importing CAD Files

You can import CAD models using the CAD readers or associative geometry interfaces (via plug-ins).

Refer to CAD Integration in the ANSYS Help for detailed CAD-related information.

For information about past, present, and future platform support, see the Platform Support section of

the ANSYS Website.

Use the File → Import → CAD... menu item to open the Import CAD Geometry dialog box, where

you can set the basic options for importing CAD files.

By default, a single file will be imported. Disable Import Single File to import multiple files and specify

the Directory and Pattern for the files to be imported.

Note

Ensure that the file path contains the appropriate platform-specific separators (for example,

C:\Tutorials on Windows systems, Home/Tutorials on Linux systems).

The following special characters are supported in the file name:

On Windows systems– + $ ^ ( ) [ ] { } @ # % _ - = , . ; ' ~ ` !

On Linux systems– + $ ^ ( ) [ ] { } @ # % _ - = , . : ; ' > “ ~ ` !

Enable Append to append CAD model data to the existing model/mesh.

Note

The Append option is available only when a model/mesh has already been read.

You can select the length unit to scale the mesh on import; models created in other units will be scaled

accordingly.The default selection is mm.

Important

The imported CAD models are scaled based on the length unit selected for the meshing

mode session only. When the model is transferred to solution mode, the model units are

reverted to the original CAD units. Refer to Scaling the Mesh (p. ) in the Fluent User's

Guide (p. ) for details on scaling the mesh in solution mode.

The following Tessellation options are available:

– If you select the CAD Faceting option, you can choose to refine the CAD faceting. Enable Refine Faceting

and specify the Tolerance for refinement and the Max Size in the CAD Faceting Controls group box.

The default value for Tolerance is , which implies no tessellation (faceting) refinement during import.

The Max Size enables you to specify a maximum facet size for the imported model to avoid very large

facets during the file import.

Importing Files

The Merge Nodes option in the CAD Options dialog box enables the merging of geometry object

nodes during CAD import. This option is enabled by default when the CAD Faceting option is

selected.

Note

→ Use the default value of  for an initial (diagnostic) import.You can then determine the

minimum size you intend to use for the mesh and import the file(s) again using a Tolerance

value /10th the intended minimum size.

→ Due to merging of nodes on geometry objects, the sizing computed at the facet nodes

may not represent the desired sizing. In this case, disable Merge Nodes in the CAD Options

dialog box and re-import the geometry objects.

– If you select the CFD Surface Mesh option, you need to specify the minimum and maximum facet sizes

(Min Size, Max Size), and the Growth Rate.

Choose the type of Size Functions to be used for creating the surface mesh.

→ By default, a Curvature size function will be used for refining the surface mesh based on the underlying

curve and surface curvature. Specify the Curvature Normal Angle to be used.

→ You can also use Proximity size functions for creating the surface mesh, based on the number of cells

per gap specified.The proximity size functions can be scoped to edges, faces, or both faces and edges.

Note that for proximity size functions, the number of cells per gap can be a real value, with a minimum

of . (see Proximity (p. ) for more information).

→ The Auto-Create Scoped Sizing enables you to create scoped sizing controls based on the

defined parameters: the scope is defined for new objects created during import. This option is

enabled by default.

→ You can also choose to save a size-field file based on the defined parameters ( Min Size, Max Size,

Growth Rate, Curvature Normal Angle, and Cells Per Gap).The size-field will be read on CAD import.

Alternatively, you can use a previously saved size-field file to create the surface mesh by enabling

Use Size Field File. Specify the Size Field File to be used.

Note

→ Mesh object nodes will always be merged when the CFD Surface Mesh is selected for CAD

import.

→ The Max Size value is limited to /10th the bounding box diagonal.

→ If you select a size-field file during CAD import, ensure that size-field file selected is appro-

priate for the length units selected.

→ Surfaces with failed surface meshes will be separated into distinct face zones and will have

the "failed" identifier in the face zone name.

→ CFD Surface Mesh options are not supported for ANSYS ICEM CFD (*.tin) files.

Selecting CAD Faceting will result in Geometry Objects on import. Selecting CFD Surface Mesh

will result in Mesh Objects on import.

The CAD Options dialog box contains additional options that can be set for importing CAD files. The

following options are available:

You can choose to read all CAD files in the subdirectories of the selected directory.

Note

CAD files with only line bodies/wires (edge zones) cannot be imported.

You can save an intermediary PMDB (*.pmdb) file in the directory containing the CAD files imported.

Note

You can use this file to import the same CAD file(s) again with different options set, for a quicker import

than the full import. A PMDB file will be saved per CAD file selected.

You can choose to process Named Selections from the CAD files, including Named Selections from

ANSYS SpaceClaim, ANSYS DesignModeler, publications from CATIA, and so on. Additional options to

ignore import of Named Selections based on pattern or by wild card are available using the

/file/import/cad-options/named-selections text command (see the Text Command

List for details).

Note

Named Selections defined in ANSYS Meshing cannot be imported.

Important

In general, names from the CAD file are retained on import. Valid characters for ob-

ject/zone names include all alphanumeric characters as well as the following special

characters:

_ + - : .

All other characters, including spaces and slashes (/), are invalid. If an invalid character

is specified, it is replaced by a hyphen (-) upon import.

– A prefix zone will be added to the object name and face zone name if the body, part,

file, or Named Selection name begins with a digit or a special character other than “_ :”.

For example, importing a file .test.agdb with the option One object per file, will

create an object named zone.test comprising the face zone zone.test.

– A suffix -sheet will be added to the object name for surface bodies imported, except for

surface bodies imported using the One Object per part option.

By default, the curvature data from the nodes of the CAD facets is imported.You can choose to disable

this, if desired.

The Merge Nodes option enables the merging of geometry object nodes during CAD import.

This option is enabled by default when the CAD Faceting option is selected. However, due to

merging of nodes on geometry objects, the sizing computed at the facet nodes may not rep-

resent the desired sizing. In this case, disable Merge Nodes and re-import the geometry objects.

Note

Mesh object nodes will always be merged when the CFD Surface Mesh is selected

for CAD import.

By default, features will be extracted from the CAD model on import.You can choose to disable this,

if desired.

Specify an appropriate value for Feature Angle. The default value is .

The Object Creation options enable you to set up object and zone granularity on import.

– Enable Create CAD Assemblies to create the CAD Assemblies tree on CAD import. It represents

the CAD tree as it is presented in the CAD package in which it was created. All sub-assembly levels

from the CAD are maintained on import in Fluent Meshing. See CAD Assemblies (p. ) for details.

You can specify CAD object and zone granularity using the options in the drop-down lists in

the Object Creation group box. You can choose to create one CAD object per body, part,

CAD file or selection imported, whereas the program-controlled option (the default) allows

the software to make the appropriate choice. This option makes a choice between per body

and per part based on whether shared topology is off or on, respectively. Similarly, you can

choose to create one CAD zone per body (default), face, or object imported.

– You can specify object and zone granularity using the options in the drop-down lists in the Object

Creation group box.You can choose to create one object per body, part, CAD file or selection

imported, whereas the program-controlled option (the default) allows the software to make the

appropriate choice.This option makes a choice between per body and per part based on whether

shared topology is off or on, respectively. Similarly, you can choose to create one face zone per

body (default), face, or object imported.

Note

For ANSYS ICEM CFD files (*.tin), set the object granularity to one object per selec-

tion.

Important

When importing multi-body parts, it is recommended that the Object Creation

option be set to one object per part or one object per file. In this case, by default,

the part names from the CAD file will not be included in the zone names or added

as a prefix to the face zone labels or region names.

Also, the Tessellation option should be set to CFD Surface Mesh to retain the

same topology as in the CAD model.

By definition, objects do not share face and/or edge zones. If the Object Creation

option is set to one object per body or one object per selection, common face/edge

zones are duplicated on import to make the objects independent.

Additional import options are available via text commands, see the Text Command List for details.

You can continue to import the CAD files, despite errors or problems creating the faceting on certain surfaces,

or other issues.

You can import part names and body names from the CAD files.You can also import enclosure and symmetry

named selections from ANSYS DesignModeler (*.agdb) files.

You can separate feature edges based on angle, connectivity, and named selections on import. Edge zone

names will have suitable suffixes depending on separation criteria, order of zones, existing zone names

and other import options selected.

You can choose to add the component (assembly or part) name to the object/zone name. By default, the

component name will be added to the object/zone name.

You can choose whether to add the part names from the CAD file to the object and zone names on import.

The default setting is auto which adds the part names to both object and zone names when object creation

granularity is set to body.When the object creation granularity is set to part or file, the part names are

not added to the zone names, face zone labels, or the region names, by default.You can also explicitly select

yes or no.

For zones without Named Selections, you can choose to inherit the object name on import.This option is

disabled by default.

When importing Named Selections, the Named Selection will be used as the object/zone name by default,

according the object creation granularity.

You can also choose to modify zone names by using part or body names as suffixes to the Named

Selections spanning multiple parts/bodies. This option is enabled by default.

By default, Named Selections are not considered when the object creation granularity is set to one object

per file.This behavior can be modified with the use-collection-names? text command.

You can also import the Named Selections as face zone labels when the CFD Surface Mesh option is selected

for Tessellation.

You can also add labels to edges connected to a single face, edges connected to multiple faces, faces

shared by bodies (double connected faces).

You can choose to remove the extension of the CAD files from the object/face zone names on import.This

option is disabled by default.

You can choose to remove the path prefix from the object/face zone names on import.The default setting

is auto which removes the path prefix from object/face zone names when the object creation granularity

is set to one object per file.You can also explicitly select yes or no.

You can also choose to modify all duplicate object/zone names by adding incremental integers as suffix.

This option is disabled by default.

Note

Compressed CAD files (for example, *.stl.zip, *.stl.gz, *.stl.bz2) cannot be imported.

Filenames with DOS style . path (shorter path) cannot be imported. Ensure that you give

the path name in full while importing the CAD files.

Virtual topology, suppressed parts/bodies, renamed parts/bodies defined in ANSYS Mech-

anical/ANSYS Meshing will be ignored during CAD import.

To import ANSYS DesignModeler files saved with blade geometry created using ANSYS

BladeModeler (plug-in for ANSYS DesignModeler), ensure that the Geometry license pref-

erence is set to ANSYS BladeModeler as follows:

.

Select Tools > License Preferences in the ANSYS Workbench menu.

.

Click the Geometry tab in the License Preferences dialog box.

.

.

.

.

If ANSYS BladeModeler is not the first license listed, then select it and click Move up

as required to move it to the top of the list.

When using the CATIA V5 Reader on Linux systems, body hierarchy information will not be

available. Only the lowest “child” labels will appear in the tree. For more information, refer

to CAD Integration in the ANSYS Help.

Tables of platform-specific supported CAD packages can be found at Linux in the CAD In-

tegration or Windows in the CAD Integration.

Meshing Problematic Imported CAD Geometries

Certain problematic imported CAD geometries (such as multiple coils wound around a centerpoint)

may not be easily meshed using Fluent Meshing due to two uncharacteristic properties:

The ratio of the surface area and the square of the bounding box diagonal is much greater than .

Projecting a point located between the coils can lead to ambiguous results due to spatial proximity.This

is especially problematic for surface meshing because the parameter-space-free approach is the most robust

approach for the majority of models in Fluent Meshing.

To avoid issues with ambiguous point projection in such geometries, use a plane to split the face of

the geometry into an upper half and a lower half:

Figure . : Splitting the Face of a Coiled Geometry

When the split model is then imported into the meshing mode of Fluent, the single volume is retained,

however the face of the volume is split and you can obtain a proper mesh because the point projection

ambiguity no longer exists,

Figure . : Imported Coiled Geometry

Graphic window displays can be saved in various formats such as TIFF, EPS, and PostScript. There can

be slight differences between pictures and the displayed graphics windows depending on your settings

and hardware, as the pictures may be generated using the internal software renderer while the graphics

windows may use specialized graphics hardware for optimum performance. To eliminate such differences

and save these files at the fastest rate possible, you must follow all of the following best practices:

Run Cortex on a suitable machine with an appropriate graphics card and the latest drivers (for details,

see the ANSYS website). Note that you can assign Cortex to a particular machine using the

gui_machine=<hostname> command line option, or by selecting Specify Machine from the

Graphics Display Machine list in the Scheduler tab of Fluent Launcher.

Ensure that Cortex / the host process is run on a separate machine than that used for compute node . For

example, do not include the machine assigned using the -gui_machine option as the first machine in

the hosts file / machine list (specified using the -cnf=x command line option).

Do not set the graphics driver to null, x11 (for Linux), or msw (for Windows).

When saving picture files, enable the Fast hardcopy option in the Preferences dialog box (under Graphics).

Saving Picture Files

Many systems provide a utility to “dump” the contents of a graphics window into a raster file. This is

generally the fastest method of generating a picture (as the scene is already rendered in the graphics

window) and guarantees that the picture will be identical to the window.

... Using the Save Picture Dialog Box

You can use the Save Picture dialog box to set the parameters and to save the picture files.

For your convenience, the Save Picture dialog box can also be opened using the Save Picture button

(

) in the standard toolbar. The procedure for saving a picture file is as follows:

.

Select the appropriate file format.

.

Set the coloring.

.

Specify the file type, if applicable (optional).

.

Define the resolution, if applicable (optional).

.

Set the appropriate options (landscape orientation, white background).

.

If you are generating a window dump, specify the command to be used for the dump.

.

Preview the result (optional).

.

Click the Save... button and enter the filename in the resulting Select File dialog box.

Tip

Click Apply instead of Save... to save the current settings without saving a picture.

The applied settings will become the defaults for subsequent pictures.

Choosing the File Format

To choose the file format, select one of the following options in the Format list: EPSEPS12, JPEG, PNG,

PostScript2, PPM, TIFF3VRML4, Window Dumps (LINUX Systems) (p. ).

(Encapsulated PostScript) output is the same as PostScript output, with the addition of Adobe Document Structuring Conventions

(v2) statements. Currently, no preview bitmap is included in EPS output. Often, programs that import EPS files use the preview bitmap

to display on-screen, although the actual vector PostScript information is used for printing (on a PostScript device). You can save EPS

files in raster or vector format.

2Raster is an optional format.

3The TIFF driver may not be available on all platforms.

4VRML is a graphics interchange format that enables export of 3D geometrical entities that you can display in the graphics window.

This format can commonly be used by VR systems and in particular the 3D geometry can be viewed and manipulated in a web-browser

graphics window. Non-geometric entities such as text, titles, color bars, and orientation axis are not exported. In addition, most display

or visibility characteristics set in Fluent, such as lighting, shading method, transparency, face and edge visibility, and outer face culling,

are not explicitly exported but are controlled by the software used to view the VRML file.

Specifying the Color Mode

You can specify which type of Coloring you want to use for all formats except VRML and the Window

Dump.

Note

Most monochrome PostScript devices will render Color images in shades of gray. Select

Gray Scale to ensure that the color ramp is rendered as a linearly-increasing gray ramp.

Choosing the File Type

When you save a PostScript or EPS file, you can choose either of the following file types:

Raster: A raster file defines the color of each individual pixel in the image. Raster files have a fixed resolution.

Vector: A vector file defines the graphics image as a combination of geometric primitives like lines, polygons,

and text.Vector files are usually scalable to any resolution.

Defining the Resolution

For raster files, you can control the resolution of the image by specifying the size in pixels. Set the

desired Width and Height under Resolution. If the values of Width and Height are both zero, the

picture is generated at the same resolution as the active graphics window.

Note

For PostScript and EPS files, specify the resolution in dots per inch (DPI) instead of setting

the width and height.

Picture Options

You can set two additional options for all picture formats except VRML and the Window Dump.

Specify Landscape Orientation (enabled, default) option, or disable for Portrait orientation.

Specify a White Background (enabled, default), or disable to use the same background as the graphics

window.

Fluent also provides options that enable you to save PostScript files that can be printed more quickly.

These options are available in the display/set/picture/driver/post-format text menu.

Window Dumps (LINUX Systems)

If you select the Window Dump format, the program will use the specified Window Dump Command

to save the picture file. For example, if you want to use xwd to capture a window, set the Window

Dump Command to

xwd -id %w >

Fluent will automatically interpret %w to be the ID number of the active window when the dump occurs.

When you click Save..., the Select File dialog box appears. Enter the filename for the output from the

window dump (for example, myfile.xwd).

To make an animation, save the window dumps into numbered files, using the %n variable.To do this, use

the Window Dump Command xwd -id %w and type myfile%n.xwd as the filename in the Select File

dialog box.

Note

Each time you create a new window dump, the value of %n increases by one, so you need

not track numbers to the filenames manually.

If you use the ImageMagick animation program, saving the files in MIFF format (the native ImageMa-

gick format) is more efficient. In such cases, use the ImageMagick tool import. For the Window

Dump Command enter the default command:

import -window %w

Specify the output format to be MIFF by using the .miff suffix at the end of the filename.

The window-dump feature is both, system and graphics-driver-specific. The commands available for

dumping windows depends on your system configuration.

Important

The window dump will capture the window exactly as it is displayed, including the resolution,

colors, transparency, for example. For this reason, all of the inputs that control these char-

acteristics are disabled in the Save Picture dialog box when you enable the Window Dump

format.

Previewing the Image

Before saving a picture file, you can preview the image to be saved. Click Preview to apply the current

settings to the active graphics window so that you can see the effects of different options interactively

before saving the image.

Chapter :Working With Fluent Guided Workflows

The Fluent Guided workflows are designed to make it easier to generate a volume mesh starting from

CAD geometries. Using the workflows, you can use the predefined steps, and add steps of your own,

that walk you through common settings in Fluent in meshing mode to quickly create a valid volume

mesh for use in the Fluent solution mode.

This chapter describes the guided workflows that are available in Fluent.

.. Getting Started with the Fluent Guided Workflows

.. Using the Watertight Geometry Workflow

.. Using the Fault-tolerant Meshing Workflow

The guided workflows are available in the Workflow tab in the Fluent graphical user interface, and can

be used to create a conformal, connected volume mesh from an imported CAD geometry.

Select the appropriate workflow from the Workflow tab. Available choices are:

Use the Watertight Geometry workflow for water-tight CAD geometries that do not require much in

the way of clean-up and modifications. See Using the Watertight Geometry Workflow (p. ) for a de-

scription of the workflow and it's tasks.

Use the Fault-tolerant Meshing workflow for more complicated non-water-tight CAD geometries that

may require some form of clean-up and modifications (for example, defects such as overlaps, intersec-

tions, holes, duplicates, etc.) This workflow can be used for both internal and external flows simulations.

See Using the Fault-tolerant Meshing Workflow (p. ) for a description of the workflow and it's tasks.

Once selected, the workflow is opened and you can proceed with working through the existing tasks,

or even creating custom workflows by adding, grouping, or removing tasks.

... Prerequisites for the Fluent Guided Workflows

... Limitations of the Fluent Guided Workflows

... Customizing Workflows

... Understanding Task States

... Operating on Tasks

... Grouping Tasks

... Editing Tasks

... Saving and Loading Workflows

... Setting Preferences for Workflows

... Getting Help for Workflow Tasks

The workflows reiy on starting with a properly defined CAD geometry, and can support geometries

that contains multiple bodies, sharing common faces, or even a single, fully enclosed body. To verify

that an assembly of bodies are fully connected, use the Force Share option in SCDM, and share any

faces that are found. If Force Share is not successful, the workflow will try to connect the remaining

unconnected faces. The workflow supports named selections from ANSYS DesignModeler (DM) as well

as groups from ANSYS SpaceClaim Direct Modeler (SCDM) if these are applied on faces (not bodies).

These entities will appear as labels in the workflow.

Important

The use of named selections (DM) and groups (SCDM), for faces surrounding openings (for

solid models) and for areas where local sizing is needed, is recommended to easily identify

these locations in the workflow. Using named selections and groups will also improve per-

sistence during design changes and improve the performance for larger models.

The workflow recognizes typical naming conventions on boundaries, such as "inlet," "outlet,"

"far-field," "symmetry," "wall," "interior," or "internal." More precisely, the changing of Fluent

boundary types based on name patterns is controlled by an advanced option, which is en-

abled by default. When enabled, the following patterns and corresponding zone types are

applied on all zones:

"inlet" maps to a velocity-inlet zone

"outlet" maps to a pressure-outlet zone

"symmetry" maps to a symmetry zone

"farfield" or "far-field" maps to a pressure-far-field zone

For internal zones (that is, internal zones shared by multiple regions), the following patterns

and corresponding zone types are applied:

"interior" or "internal" maps to an internal zone

"wall" maps to a wall zone

"fluid" or prefixes using "enclosure" or "air" map to a fluid region

Using these naming conventions on boundaries will, by default, cause them to be assigned

to corresponding Fluent zone types. Consequently, it is not recommended to use any of

these naming conventions within file names or within bodies or parts in the model. Similarly

the use of "fluid" or "enclosure" is, by default, used to identify fluid regions on bodies.

Consequently, it is not recommended to use these naming conventions within boundary

names. In addition, the use of "unknown" should also be avoided.

Note

Zone names and their listings in various tasks may differ slightly from previous releases,

impacting journal files and workflow template (.wft) files that reference specific zone

Working With Fluent Guided Workflows

names. In such cases, journal files and template files will not function, and you will need to

replace the old zone names with the new version of the zone names.

Note

Note

Field-level user assistance (available by hovering next to a field and clicking on the field's

exposed help icon) is available for many fields of the workflows, however, it is not available

on Linux.

Watertight Geometry Workflow Limitations

The following limitations have been observed in the Fluent Watertight Geometry workflow:

In order to revert and edit any up-to-date task in another session or on another computer system

(such as generating a volume mesh), you will need to have the CAD geometry file available, as

well as the correct CAD configuration, and the tasks will be updated from the Import Geometry

task.

Multiple periodic systems are not supported in the workflow.

Using labels in the capping, local sizing, update boundaries, and the modify mesh refinement tasks

will be persistent during design changes, whereas using zones in these tasks is not likely to be persistent.

In addition to the display options provided in the workflow, you can use the display options of the

Ribbon and Outline View tree to visualize various regions, zones, labels, edges, objects, etc.

The workflow only supports a single mesh object. Non-conformal or overset mesh setup is not suppor-

ted.

If you need to perform changes to the topology, geometry, or the mesh, then you should incorporate

them into the workflow using the custom journal task in order to make the changes persistent in the

Fluent workflow. See Customizing Workflows (p. ) for more information.

The following tasks and categories have their own corresponding limitations:

– Import Geometry

→ You can only import CAD geometries - .stl and .tgf or .msh files are not supported.

→ The workflow only fully supports the appending of bodies used for a body of influence using a

custom journal.

– Add Local Sizing

→ The workflow supports the reading of an external .szcontrol file for advanced size control,

provided that the size field is also imported or computed within the Custom Journal task.

– Create Surface Mesh

→ When the Shared Topology task is used, the following advanced options for the Create Surface

Mesh task are actually performed at the end of the Shared Topology task:

Automatic zone separation

Getting Started with the Fluent Guided Workflows

Automatic remesh to remove clustering

Final surface mesh improvement

– Set Up Periodic Boundaries

→ Automatic periodicity is not supported if all periodic faces are non-planar.

– Apply Share Topology

→ The gap between two bodies should not exceed / of the local mesh size on the faces of the

gap.

→ The share topology success rate is increased if faces across gaps are parallel.

– Add Boundaries

→ Faces added to a label are always merged.

– Surface Remesh

→ Support body of influence (BOI) created in local sizing.

– Boundary Layer Settings

→ The boundary layers settings are applied on all fluid region walls.

– Volume Mesh Settings

→ The workflow supports the reading of external .pzmcontrol files, and custom journals, for

advanced boundary layer settings

→ You cannot use different volume mesh types on different regions.

→ Persistent renaming only ensures persistence if unique body names are used.

– Drawing the Volume Mesh

→ To show the location of the worst volume cell, you must use the Display Grid option in the Display

menu.

– Modify Mesh Refinement

→ Refinement uses the existing mesh (and not the geometry) as the geometry on which the mesh

is refined. Hence, features that are not well captured (from a geometry standpoint) cannot be

improved upon.

– Named Selections on Multiple Bodies

→ When a Named Selection is defined on multiple bodies, the workflow recognizes the name but

not that the group should be merged into a single region.The separation of the bodies into indi-

vidual cell zones also separates boundary zones which can increase the number of zones consid-

erably for complex models.

Limitations for Using the Poly Hexcore Volume Fill Method in Parallel

– The mesh quality may not be perfect, due to a few invalid cells, and the change in size could be

large for a few cells in the poly transition area.

– Surface meshes with point contacts and edge contacts might lead to system failure.

Fault-tolerant Meshing Workflow Limitations

The following limitations have been observed in the Fluent Fault-tolerant Meshing workflow:

Import CAD and Part Management

– When importing JT CAD data, the JTOpen option is available on more recent Linux OS variants

(requiring a glibc supplying 'memcpy@GLIBC_2. '), that is, it is not supported on Red Hat /

CentOS  series.

– When importing CAD data via the Workbench route on Linux, the SLES  platform is not supported.

– Importing polyhedra and poly-hexcore mesh files is not supported.

– Importing CAD files is not supported when using remote Linux nodes from Windows.

Extract Edge Features

– When using the Intersection Loops extraction method, each object can participate only once for

any given edge grouping (that is, objects are not available to share with separate groupings). For

example, given two tire objects (tire-, and tire-) and a tunnel object (tunnel-) with

which they intersect; you can create an edge group for tire-, tire-, and tunnel- collectively.

You cannot, however, create individual edge groups that share tunnel- (for example, a grouping

of tire- and tunnel-, and a separate grouping of tire- and tunnel-).

Generate the Surface Mesh

– The workflow does not support adding zone-specific settings (such as boundary layers) after the

Generate the Surface Mesh task.

Preferences

– The workflow does not fully support the Write into memory option, so if selected as a preference,

the workflow will use Write mesh files instead. See Setting Preferences for Workflows (p. ) for

more information about preferences in saving data for editing tasks.

– Only  mesh object is supported. One cannot mesh multiple mesh objects.

– Using poly for the wrapper type surface mesh may generate a few poor quality or invalid cells. For

a better quality CFD surface mesh, use the Watertight Geometry workflow.

By default, the guided workflows consist of several existing tasks that represent common operations

for mesh preparation. In addition, you can add and remove certain tasks as needed, depending on

where you are in the workflow, and the specific level of complexity for your own desired workflow.

Each task requires certain inputs and provides certain outputs that other tasks may depend upon, so

only certain task may be available to add to the workflow, depending on previous tasks.

The tasks available for the Watertight Geometry workflow are described in Using the Watertight

Geometry Workflow (p. ), whereas the tasks available for the Fault-tolerant Meshing workflow are

described in Using the Fault-tolerant Meshing Workflow (p. ).

The following tasks can be added to a workflow multiple times:

Update Regions

Add Boundary Type

Update Boundaries

Run Custom Journal

Customized workflows can be saved and reused later. For more information, see Saving and Loading

Workflows (p. ).

Standard journals (Creating and Reading Journal Files (p. )) are supported in the workflows as well.

While using the workflows, only the values that you change are recorded in the journal, making them

cleaner and easier to read. Any workflow-related commands use the workflow prefix. For example:

...

(%py-exec "workflow.InitializeWorkflow(WorkflowType=r'Watertight Geometry')")

(%py-exec "workflow.TaskObject['Import Geometry'].Arguments.setState({r'FileName': r'D:/sample/elbow.scdoc',})")

...

(%py-exec "workflow.TaskObject['Import Geometry'].Execute()")

...

(%py-exec "workflow.TaskObject['Describe Geometry'].Execute()")

(cx-use-window-id )

(cx-set-camera-relative '(. . -.) '(  ) '(-. -. -.) )

(%py-exec "workflow.TaskObject['Create Regions'].Arguments.setState({r'NumberOfFlowVolumes': ,})")

...

Customized journal files can be created and added to either workflow (Running Custom Journal

Commands (p. )). The following example demonstrates a customized scoped prism control file for

boundary layers. The example creates prism controls and sets various properties such as the name,

type, first height, etc.

(

("fuselage-prisms" "last-ratio" . . "fluid-" "fluid-regions" "" "selected-face-zones" "*fuselage*")

("rest-prisms" "last-ratio" . . "fluid-" "fluid-regions" "" "selected-face-zones" "*fin* *pylon* *pod* *w

)

Tasks in the workflow tree can have four states:

Tasks that are complete are indicated by a green check mark icon (

).

Tasks that are complete but contain warnings are indicated by a green check mark icon with an asterisk

(

).Tasks with this icon have one or more problematic property settings, however Fluent will still

allow you to proceed with defining other tasks in the workflow.The console window may contain in-

formation about the details surrounding the problem. Right-click the task while in this state and select

Show Errors and Warnings to display a dialog the will outline the problems identified with this task.

Tasks that are incomplete are indicated by a lightning bolt icon (

).

Tasks that require attention are indicated by an exclamation point icon (

).Tasks with this icon have

one or more problematic property settings that require your attention before proceeding further in

the workflow.The console window may contain information about the details surrounding the problem.

Right-click the task while in this state and select Show Errors and Warnings to display a dialog the

will outline the problems identified with this task.

You can perform various operations on a task in the workflow tree by right-clicking the task in the

tree and using the context menu to:

Add new tasks to the workflow by choosing Insert Next Task.The available tasks that can be inserted

are arranged by what is recommended.

Group tasks together by selecting them and choosing Create Group.

Complete, or execute, a task by choosing Update.

Delete a task by choosing Delete.

Rename a task by choosing Rename.

The ability to automatically display a task's objects in the graphics window (such as mesh elements,

facets, etc.) is disabled for larger models when using the Fault-tolerant Meshing workflow, depending

on the Task based display preference setting (see Setting Preferences for Workflows (p. )). If a task

has a particular display available, you can display objects for that task in the graphics window by

hovering over the task in the workflow tree and selecting the

icon that appears. This is useful to

quickly visualize a task's objects without having to explicitly visit the task details.

In addition to using the provided tasks, you can create your own custom group tasks using the Create

Group command on the context menu in the workflow. A group task is a collection of standard tasks

that you have collected and grouped together.

When you update a group task, the system updates all of the tasks within the group sequentially, while

standard tasks can only be updated once (without being edited), a group task can be updated at any

time.

When a task is complete and up-to-date, all controls within that task are disabled. If you need to make

any changes to any of your settings within the task, enable the task's controls by clicking the Edit

button within the task (or click Edit in the context menu from the workflow tree). Once you have made

your changes, clicking Update restores the task's state (causing all subsequent up-to-date tasks to

then become out-of-date) and updates the current task with its new changes. Downstream tasks will

remain out-of-date until you update them manually. If you decide to select Cancel, then all changes

are discarded and the task's state will remain up-to-date.

Some tasks include zone or label selection lists where you have made a selection. To edit such tasks,

enable the task's controls by clicking the Revert and Edit button (or click Revert and Edit in the

context menu), thereby reverting to the task's previous state, and causing all subsequent up-to-date

tasks to then become out-of-date. Once you have made your changes, clicking Update then updates

the current task with its new values. If you decide to select Cancel, then all changes are discarded and

the task's state is not restored. The current task and all downstream tasks will remain out-of-date until

you update them manually.

As you progress through using the workflows, you can save them at any time using the Save Workflow

button (

). When you save the workflow itself, you save the tasks, sub-tasks, and their settings, as

your own custom workflow template for future use. You can also load any saved workflow using the

Load Workflow button (

). If you make a mistake in setting up your workflow, you can delete the

task (using the Delete command in the context menu for the selected task), or even reset the entire

workflow (using the Reset Workflow button (

)).

It should be noted that when you write the mesh file (File > Write > Mesh...), Fluent saves the current

workflow along with any mesh information within the saved mesh file.

Note

Workflows are saved as workflow template files (using the *.wft file extension). The *.wft

files include the version number of the current release (for example, for the  R3, release,

the files are internally designated with "version": ". ".

You can access global preferences when using guided workflows in Fluent through the Preferences

dialog.

Through the Meshing Workflow category, the Preferences dialog contains global settings that are

useful when working with guided workflows:

dialog.

For Saving data for editing tasks, you can determine how mesh files are managed when you

edit your workflow tasks. Choices include:

– Use the Write mesh files option to save a mesh file into a temporary folder while editing

mesh-related tasks within the workflow.

→ When this option is enabled (the default), Fluent creates a mesh file for use when a com-

pleted mesh-related task needs to be edited.

→ When this option is disabled, Fluent will not create a mesh file, and when the completed

mesh-related task needs to be edited, Fluent automatically updates each previous task in

order to generate the required mesh file.

Disabling this preference is recommended if you do not need to edit your workflow

tasks once they have been defined.

– Use the Write into memory option to save mesh file information to memory while editing

Note

The Fault-tolerant Meshing workflow does not fully support the Write into

memory option, so if selected as a preference, the workflow will use Write

mesh files instead.

– Use Do not save data to not save a mesh file while editing a task.

Note

If the Saving data for editing tasks option is set to Do not save data, and

you are reverting any changes to a particular task, then updating that task

subsequently updates all previous tasks.

Whether the Saving data for editing tasks option is set to Write mesh files

or Write into memory, mesh information is saved for a particular task when

the task is completed. When you choose to edit any settings to a completed

task, the saved mesh information corresponding to that task is retrieved and

the task's settings are restored accordingly.

See Editing Tasks (p. ) for more information reverting and updating task.

Use the Temporary files folder field to control where Fluent will write the temporary mesh files

generated while using the workflows.You can specify a valid location, or by default, the location is

set to the %TEMP% folder on Windows and to the /tmp directory on Linux.

Use the Verbosity option to determine whether or not you see task-related messages in the console

window that might assist you with your workflow.The default is off which limits the output to the

console.

Use the Task based display option under Graphics Settings to control how Fluent automatically

displays items in the graphics window within the tasks of the workflow.

– A value of auto will automatically display objects (or refinement regions, edge zones, size

boxes, etc.) in the graphics window within the task, based on the threshold values defined

for the Automatic display face zone limit and the Automatic display facet limit.

– A value of yes will always automatically change displayed objects in the graphics window

within the task, according to the task's display requirements.

– A value of no will never automatically change displayed objects in the graphics window,

throughout the entire workflow.

You can access general and task-specific documentation for the workflows and the associated tasks

by selecting the Workflow Help button (

). In addition, the workflows include user assistance for

most fields without leaving the workflow, available by hovering next to a field and clicking on the

field's exposed help icon.

This section describes the various tasks that are provided when using the Watertight Geometry guided

workflow:

... Importing CAD Geometries

... Adding Local Sizing

... Creating Surface Meshes

... Setting Up Periodic Boundaries

... Describing the Geometry

... Applying Share Topology

... Enclosing Fluid Regions

... Creating Regions

... Updating Regions

... Creating a Volume Mesh

... Updating Boundaries

... Improving the Surface Mesh

... Adding Boundary Types

... Improving the Volume Mesh

... Modifying Mesh Refinement

... Running Custom Journal Commands

Use the Import Geometry task to designate a CAD geometry for your simulation.

. Choose a suitable option for the Units. It is recommended to work in units where the minimum size of

the mesh is of the order of one.The mesh will automatically be scaled to meters while transferring the

mesh to the Fluent solver

. Click Advanced Options to access additional controls prior to performing this task. Options include:

Use the Separate Zone By option to determine how zones are separated, either by region alone, by

region as well as a specified separation angle, or neither. Zone separation is necessary if local sizing

needs to be applied. Region separation is sufficient for body sizing and/or body of influence, while

separation by angle is needed for local face sizing.

When Separate Zone By is set to region & angle, set the Separation Angle to a value for which

CAD zones are separated. The lower the value for the angle, the higher the number of faces that

will be separated. The default value is  degrees.

Note

If you are separating zones by angle, and if a body of influence (BOI) is part of the

model, you must create a face-based named selection or group for the BOI using DM

or SCDM so that you are able to select and add the BOI in the Add Local Sizing task

(see Adding Local Sizing (p. )).

Set the Tolerance (% of min-size) value, determining the level of facet refinement during import.

It is recommended to use a value around % of the intended minimum size. Using a value of  results

in the coarsest possible faceting.

Set the Max Facet Length value to avoid very large facets during file import.

. Browse for a specific File Name.

Supported file types are SpaceClaim (.scdoc) and Workbench (.agdb) files and also .pmdb files.

Note

When a SpaceClaim (.scdoc) file is imported into Fluent while in meshing mode, Fluent

also creates an intermediary .pmdb file that can be imported. The .pmdb file should

always reside alongside the .scdoc file. When changes are made to the geometry in

SpaceClaim, and the file is reimported into Fluent, the original .pmdb file is overwritten.

The .pmdb file can be more easily and quickly read into Fluent for additional processing.

Note

SpaceClaim (.scdoc) files are only supported on Windows. When working on Linux

systems, however, you can use the intermediary .pmdb file as your geometry file for

Note

the workflows.

On Windows, use the Import CAD Geometry dialog to import the CAD file into Fluent,

and enable the Save PMDB (Intermediary File) option in the Import Options dialog.

After the file is imported, you can move the generated .pmdb file over to your Linux

system to use in your workflow.

. If you have manually entered a CAD geometry file name, click Import Geometry, otherwise the task is

automatically performed if you browse and select a CAD file.

If you need to make adjustments to any of your settings in this task, click Edit, make your changes

and click Update, or click Cancel to cancel your changes.

. Proceed to the next step in the workflow.

Using the Watertight Geometry Workflow

You can gain better control over the mesh size distribution by using the Add Local Sizing task. Using

this task, you can define specific mesh size controls that operate on specific, localized, portions of the

geometry and mesh. Using this task, you can add as many localized size controls to the workflow as

you need, depending on the requirements and details of your geometry. Note that this task can only

be added to the workflow prior to the Create Surface Mesh task.

For the Would you like to add local sizing? field, select yes if you need to define local sizing para-

meters using the following steps. Otherwise, if you do not need to define local sizing controls, keep

the default of no, click Update and proceed to the next task.

. Provide a Name for the new size control, or use the default name. The default name changes de-

pending on the assigned Size Control Type.

. Provide a Growth Rate.

. Choose the Size Control Type. Choices include:

Use the Face Size setting for refining the local sizing based on the face size.

Use the Body Size setting for refining the local sizing based on the body size.

Use the Body of Influence setting, or BOI, to assign a maximum size on all parts of your geometry that

falls within the boundaries of the body of influence.

Note

For a body that is associated with a Body of Influence (BOI body), keep the following

in mind:

– The BOI body must not share topology with the CAD model itself within SCDM or

DM.

– The BOI body must have a unique name within SCDM or DM.

– All imported BOI bodies must be assigned a local sizing control.

Use the Curvature setting for refining the local sizing based on the underlying curve and surface

curvature.This size control type is useful, for instance, in models with a combination of large and small

scales.

Use the Proximity setting for refining the local sizing based on the number of cells per gap specified.

. If you are using the Face Size, Body Size, or Body of Influence size control type, provide a Target Mesh

Size.

Note

Clicking in this field displays red boxes in the graphics window, providing a visual rep-

resentation of the field value. Use the Clear Preview button to hide the visualization

display.

. If you are using the Curvature size control type, you have the following options:

Specify a value for the Local Min Size for the curvature size control.

Specify a value for the Max Size for the curvature size control.

Specify a value for the Curvature Normal Angle for the curvature.

Specify a value for the Scope to field, where you can localize the size control to faces, edges, or faces

and edges. Edge selection selects the edges of a particular face.

. If you are using the Proximity size control type, you have the following options:

Specify a value for the Local Min Size for the proximity size control.

Specify a value for the Max Size for the proximity size control.

Specify a value for the Cells Per Gap.This value is the number of element layers to be generated in a

gap for the edge proximity size function. Note that for proximity size functions, the number of cells per

gap can be a real value, with a minimum value of .. See Proximity (p. ) for more information.

and edges.

. You can select an available zone or label to apply your local sizing changes. Choose whether to Select By

the zone name, or the label name in the list below.

If you Select By labels, in the Face Zone Labels list, you can choose a label in the list, or enter text to

filter out the available labels in the list before selecting a label.

Note

Labels originate from the CAD geometry, such as from group names in SpaceClaim

geometries, or from named selections in DesignModeler geometries.

If you Select By zones, in the Face Zones list, you can choose a zone in the list, or enter text to filter

out the available zones in the list before selecting a zone.

. Click Add Local Sizing.

You can add as many local sizing controls as you require for your workflow, each operating on

different zones and/or with different sizing parameters. The size controls will appear as sub-tasks

under the parent task.

If you need to make adjustments to any of your settings in this task, select the specific size control

sub-task, click Revert and Edit, make your changes and click Update, or click Cancel to cancel

your changes.

Note

If you need to add another local sizing control after you have already created a surface

mesh, you need to revert and edit at least one existing local size control in order to

properly see and use the available geometry objects in the graphics window and the

object listing. Alternatively, you can also re-import your geometry and update the Add

Local Sizing task.

. Once you are satisfied with your changes, proceed to the next step in the workflow.

Use the Create Surface Mesh task to create a conformal, connected surface on all of the objects in

the geometry, and identify regions that will later be filled with the volume mesh. In many cases, the

default values will be sufficient for a useful CFD surface mesh.

. Set the Minimum Size of the facets for the surface mesh.

Note

display.

. Set the Maximum Size of the facets for the surface mesh.

Note

display.

Note

display.

. Specify the Growth Rate.

. Choose a Size Function.

The Curvature size function can be used for refining the surface mesh based on the underlying curve

and surface curvature.

The Proximity size function can be used for creating the surface mesh, based on the number of cells

per gap specified.

By default, a Curvature and Proximity size function is assigned based on both curvature and proximity.

For additional information, see Size Functions and Scoped Sizing (p. ).

. For the Curvature or the Curvature and Proximity size functions, specify the Curvature Normal Angle

for the curvature size function.The default value of  degrees should approximately produce  facets

in the circumferential direction of a cylinder.

. For the Proximity or the Curvature and Proximity size functions, specify the Cells Per Gap for the

proximity size function.This value is the number of element layers to be generated in a gap for the edge

proximity size function. Note that for proximity size functions, the number of cells per gap can be a real

value, with a minimum value of .. See Proximity (p. ) for more information.

. For the Proximity or the Curvature and Proximity size functions, choose the Scope Proximity To value

for the proximity size function, which can be scoped to edges, faces, or both faces and edges.

. Click Advanced Options to access additional controls prior to performing this task. For additional inform-

ation, see Face Connectivity Issues (p. ) and Quality Checking (p. ). Options include:

Use the Check Self-Intersection? field to determine whether or not the system will check for self-inter-

secting faces as part of the surface mesh creation.This check will, for example, detect if share topology

has been omitted. For larger models, this check, however, can be time consuming, so if a model initially

passes this test the first time, it can be safely disabled.

Figure . : Example of a Self-Intersection: Double Faces Appear When Share Topology is

Not Enabled

Figure . : Example of a Self-Intersection: Local Mesh Size is Significantly Larger Than the

Pipe Thickness

Use the Limit for Smoothing Folded Faces option to provide a value limiting when folded faces are

resolved during surface mesh creation.

Use the Invoke Zone Separation by Angle? option to determine whether or not to separate zones. If

set to yes, separation is based on a specified separation angle. Separation is needed for operations

such as flow volume extraction and mesh refinements, in cases where named selections have not been

defined in advance inside the CAD model.

Use the Separation Angle option to specify a desired angle for determining separation. Assigning a

smaller separation angle will produce more zones.

Use the Auto Assign Zone Types? option to automatically assign inlet, outlet, internal, and symmetry

boundary types to zones during surface mesh creation.

Use the Invoke Quality Improve? option to choose whether or not quality measures are applied during

surface mesh creation. Surface mesh quality improvements should be invoked after importing the CAD

model.

– When Invoke Quality Improve? is enabled, an attempt will be made to improve the quality on those

triangles where the skewness is above the Quality Improve Skewness Limit.

Note

If local sizing has been added, these curvature and proximity size controls are ap-

pended to the local sizes and the resulting size field is used to dictate the sizes

during surface meshing.

– When Invoke Quality Improve? is enabled, four consecutive attempts are made to improve the

quality, each using a larger adjacent angle, until the Quality Improve Max Angle.

– When Invoke Quality Improve? is enabled, and after quality improvements, using the Quality Im-

prove Skewness Limit and Quality Improve Max Angle are complete, if any remaining triangles

are above the Quality Improve Collapse Skewness Limit value, these triangles will be aggressively

removed using a fixed maximum angle of  degrees.

Use the Auto Remesh to Remove Clustering? option to automatically remesh the surface mesh to

remove excessive clustering of nodes. Using the default will only invoke this automatic remesh if the

Add Local Sizing task has been added to the workflow.

. Click Create Surface Mesh to generate a CFD surface mesh for the imported CAD geometry.

During the process of creating the surface mesh for an imported CAD assembly geometry containing

multiple parts, Fluent can detect whether or not the geometry has shared topology enabled. If the

imported geometry does not have shared topology enabled, Fluent will provide your workflow

with a Shared Topology task (within the Describe the Geometry task, see Applying Share Topo-

logy (p. )) where you can identify and close any problematic gaps and choose whether to join

and/or intersect the problematic faces.

When the Shared Topology task is used, the following advanced options for the Create Surface

Additional quality improvements can be made to surface meshes using the Improve Surface Mesh

task (see Improving the Surface Mesh (p. )).

You can use the Set Up Periodic Boundaries task to define rotational and/or translational periodicity

in your simulation. This task essentially re-meshes a single periodic face to exactly match the reference

side of the face, as well as define the corresponding Fluent boundary types (periodic and shadow), in

preparation for the Fluent solver. If your periodic simulation also involves shared topology (Applying

Share Topology (p. )), you should first invoke the Apply Share Topology task prior to the Set Up

Periodic Boundaries task.

. Use the Type field to choose whether you are creating rotational or translational periodic boundaries.

. Use the Method field to choose how you are going to define your periodic boundary.

Choose Automatic - pick both sides to define the periodic boundary based on your zone/label

selections

Note

When using this option, you must select two zones or labels.

Choose Manual - pick reference side to manually assign properties of the periodic boundary.

Note

When using this option, you only need to select a single zone or label.

You would use this option in the following situations:

– You already know the periodicity angle, or translational shift, the components of the origin,

and the components of the vector, and which side is the reference side.

– All your periodic faces are non-planar.

– The mesh is asymmetric on the two periodic faces, and you need to use the side with the

refined mesh as a reference.

For rotational periodicity:

a.

Specify a value for the Periodicity Angle.

b. For the Origin Components, specify a value for X, Y, and Z.

c.

For the Vector Components, specify a value for X, Y, and Z.

For translational periodicity, under Translational Shift, specify a value for X, Y, and Z.

. Choose whether to Select By the zone name or the label name in the list below.

If you Select By zones, in the Zones list, you can choose a zone in the list, or enter text to filter

If you Select By names, in the Labels list, you can choose a label in the list, or enter text to filter

out the available labels in the list before selecting a label.

Note

. Once your selections are made, click the Set Up Periodic Boundaries button and proceed to the

next task.

Once the task is completed, you will see an indicator in the graphics window showing the

origin and vector, as well as updated mesh, where you can verify that the periodic sides have

identical meshes. When the automatic option is used, the console displays the calculated

periodicity angle, origin components, and vector components for future reference.

If you need to make adjustments to any of your settings in this task, click Edit, make your

changes and click Update, or click Cancel to cancel your changes.

Note

If you return to the Set Up Periodic Boundaries task after creating a volume mesh,

you can restore the visibility of the mesh by using the F2 hot key and either the

Fit to Window icon (

) or the Draw Mesh button at the bottom of the task.

The Watertight Geometry workflow uses the Describe Geometry task to let you specify the type of

geometry you are importing: whether it is a solid model, a fluid model, or both. Settings in this task

determine what sub-tasks are available for the overall task.

. For the Geometry Type, choose from the following:

The geometry consists of only solid regions: for solid models, you are provided with sub-tasks

related to creating capping surfaces over any openings in the geometry, and calculating regions.

The geometry consists of only fluid regions with no voids: for fluid models with no pockets,

you are provided with a sub-task for updating boundaries.

The geometry consists of both fluid and solid regions and/or voids: for geometries with both

a solid and a fluid, and potential pockets, you are provided with sub-tasks related to creating

capping surfaces over any openings in the geometry, updating boundaries, and calculating regions.

. Indicate whether or not your goal is to cover any openings in your geometry and to extract a fluid

region.

. Indicate whether or not you want to have Fluent convert all fluid-fluid boundary types from 'wall' to

'internal'.The default is No, however, if you select Yes, Fluent will convert all interior boundary types

from walls to internal boundaries. Named selections that include the string "wall" are excluded from

this conversion.

. Once your selections are made, click the Describe Geometry button and proceed to the next task.

imported geometry does not have shared topology enabled, Fluent will provide your workflow with

an Apply Share Topology task (within the Describe the Geometry task) where you can identify and

close any problematic gaps and choose whether to join and/or intersect the problematic faces.

In an assembly, each individual body contains all of its faces, none of which are shared with another

body, thus making the model "non-conformal" to Fluent, where special handling is required for the

solver. By performing the Apply Share Topology task, all bodies in contact will share faces across

bodies, and the model is made "conformal" thus making the model compatible with the Fluent solver.

Note

When ANSYS SpaceClaim DesignModeler cannot perform a Force Share operation, the

problematic faces are identified as specifically named selections (for example, Connect

Topology  or Connect Topology , and so on). You can use such partially

shared topologies within the workflow, however, you must retain those specifically named

selections - you should not remove or rename them.

. Specify a value for the Max Gap Distance.

. Click the Show Marked Gaps  button to identify gaps that are less than the gap distance.

Note

The Max Gap Distance should be equal to or less than half of the value specified

for the Minimum Size in the Create Surface Mesh task. Also, the Max Gap Distance

should never exceed the thickness of a solid or fluid body, otherwise the solid or

fluid bodies may potentially collapse.

Note

You should be cautious when setting an appropriate Minimum Size for the surface

mesh. Using an unnecessarily small minimum size value, relative to the gap distance,

Note

may cause problems generating a successful Share Topology task.

See Troubleshooting Gap Marking (p. ) for more information.

Use the Join Pair Normal Angle option to specify the feature angle to identify features in the

overlap region.

Use the Initial Relative Join Tolerance option to specify the tolerance value (relative to face

edges) for locating the overlapping faces.

Use the Number of Join Attempts option to control the number of times the task attempts to

join faces within the gap.

Use the Join Tolerance Increment option to control the change in tolerance with each join attempt.

Use the Join and Intersect Method option to control whether the gap faces are joined, whether

they are intersected, or both.

Note

The Initial Relative Join Tolerance can be aggressive, in relation to the Number

of Join Attempts, so increasing the number of attempts may yield better results

for certain circumstances. In addition, improvements are possible if you cross-imprint

overlapping faces within SpaceClaim so that you have one-to-one face matching.

. Once your selections are made, click the Apply Share Topology button and proceed to the next

task.

The task locates and joins problematic face gaps and intersections through a series of incre-

mental attempts until the geometry exhibits the equivalent of shared topology.

....Troubleshooting Gap Marking

In the Shared Topology, use the Show Marked Gaps button to display any gaps in the geometry

less than the Max Gap Distance size. Gaps between object pairs are identified and highlighted in

Figure . : Showing Marked Gaps

Once marked, you can select the Apply Share Topology button to update the task and view the final

results. Based on the task's default settings, pairs are processed and joined and/or intersected according

to various tolerances over a number of incremental steps, until all identified pairs are successfully

processed and all gaps between parts are closed.

Figure . : Applying Share Topology to Marked Gaps

In some cases, sporadic gap markings are possible when the Max Gap Distance is not sufficient:

Figure . : Incomplete Gap Marking (Max Gap Distance = .)

Improvements can be made by adjusting the Max Gap Distance accordingly.

Figure . : Complete Gap Marking (Max Gap Distance = .)

Additionally, using a value for the gap distance that is too aggressive may lead to a collapse of the

geometry entirely once the task is updated.

Figure . : Excessive Gap Marking Around a Washer (Max Gap Distance = .)

Slight readjustments of the Max Gap Distance in accordance with the minimum size can be successful:

Figure . : Proper Gap Marking Around a Washer (Max Gap Distance = .)

In some case, you may be required to adjust and re-adjust the value of the Max Gap Distance field

so that all gaps are properly identified and closed.

For solid model geometries, you can use the Enclose Fluid Regions (Capping) task to cover, or cap,

any openings in your geometry in order to later calculate your fluid region(s).

. Specify a Name for the capping surface, or use the default name. The default name changes de-

pending on the assigned Zone Type.

. Choose the Zone Type for the new cap. Choices include:

velocity-inlet

pressure-outlet

pressure-inlet

pressure-far-field

mass-flow-inlet

outflow

symmetry

wall

. Choose whether the Cap Type will be based on a single surface opening, or if it is an annular opening

with two surfaces.

Note

A single surface opening can potentially have more than one face comprising the single

surface:

Figure . : Example of a Single Surface Cap with Multiple Faces

A single surface opening can also mean selecting multiple, distinctly separate, surfaces

to create a single cap:

Note

A single named selection using both the inner and outer face is the only valid selection

for annular capping using labels.

Figure . : Example of an Annular Cap Type

Note

The workflow does not support tilted annular faces for capping (highlighted in red, be-

low). Currently, two caps are created (highlighted in green, below) and the resulting

intersecting cap must be manually removed,

Figure . : Example of a Problematic Tilted Annular Opening

If you Select By zones, in the Zones list, you can choose a zone in the list, or enter text to filter out the

available zones in the list before selecting a zone.

If you Select By names, in the Labels list, you can choose a label in the list, or enter text to filter out

the available labels in the list before selecting a label.

Note

Use the Check Cap Self-Intersection? option to control whether or not the system will detect if the

capping surface intersects with any other face in the model. If an intersected face is found, it is automat-

ically deleted.To increase the efficiency of the capping task, this option should be set to no.

Figure . : Example of a Self-Intersection: Additional Cap Intersects With Other Surfaces

Use the Max Cap Edge Count Limit option to control the number of edges that can be present on the

capping surface.

. Click Enclose Fluid Regions (Capping).The new capping object will appear in the workflow and in the

graphics window.

In cases where a face has multiple holes, and only a portion of them will be used for fluid extraction,

Fluent will cap all holes on the face, and will only use the capped openings that are required for

extracting the fluid region.

If you need to make adjustments to any of your settings in this task, click Revert and Edit, make

your changes and click Update, or click Cancel to cancel your changes.

. Repeat as needed for additional inlets, outlets, etc., until all openings have been assigned a type and have

been created.

. Once all openings have been covered, proceed to the next step in the workflow.

You can specify the number of fluid regions to be included in your simulation using the Create Regions

task.

. Choose the number of fluid volumes you wish to create in the Estimated Number of Fluid Regions field,

or use the default value.

Note

The system will detect additional regions if they exist, however, it will detect fluid regions

only where they are connected to capping surfaces.

By default, all bodies are solid regions and all voids are considered "dead" regions. The conversion

to a fluid region can happen in many ways:

There is a named selection matching *fluid* or *enclosure* or air*.

Any region sharing a boundary with any of the inlet or outlet boundary types will automatically

changed to fluid region.

Any region sharing "internal" boundaries will also change to "fluid" region.

When compute regions occurs the estimated value are based on existing fluid regions.

. Click Create Regions.

Note

Once this task is completed and updated, if fluid extraction is required, Fluent will display

the newly created fluid regions.

Note

. Use the Draw Regions button to display the available regions in the graphics window.

. When the flow volume is generated, proceed to the next step in the workflow.

For solid models, you may proceed to the Create Volume Mesh task.

Additional enhancements can be made to regions using the Update Regions task (see Updating Re-

gions (p. )).

You can update the properties of any defined region using the Update Regions task. This task can

be added to the workflow as many times as you require.

The table contains a list of all of the defined regions, and their assigned types.

. (optional) Use the Filter button to filter the table contents based on a particular column.

. Assign a Region Name as needed by double-clicking the current name.

You can also rename one or more regions by selecting them in the table, right-click, and select Set

Region Name in the context menu, and provide a new name directly in the menu.

. Assign a Region Type as needed using the corresponding drop-down menu. Available region types include:

fluid

solid

dead

Note

Dead regions are the same as a void or a pocket in the domain, and are not transferred

to the Fluent solver.

Multiple regions can be assigned a specific type all at once by selecting them in the table, right-

click, and select Set Region Type in the context menu, then designate a type for the selected

regions directly in the menu.

Multiple regions can be visualized all at once by selecting them in the table, right-click, and select

Draw Selections in the context menu.

. When you are satisfied with the region assignments, click Update Regions.

. Once all regions have been updated, proceed to the next step in the workflow.

You can generate a computational mesh for your fluid volume(s) using the Create Volume Mesh task.

In many cases, the default values will be sufficient.

The Create Volume Mesh task actually performs two separate operations: creating the boundary layer,

as well as the creating the volume mesh.

Boundary layers are automatically added upon all the boundaries of all fluid regions, except on any

boundaries for which a boundary condition (inlet, outlet, symmetry, internal) has been applied. On

these boundaries, the boundary layers will be imprinted on the face.

. Provide boundary layer settings. See Prism Meshing Options for Scoped Prisms (p. ) for more information.

a.

Choose an Offset Method Type.The offset method that you choose determines how the mesh cells

closest to the boundary are generated. See Offset Distances (p. ) for more information. Choices in-

clude:

aspect-ratio: allows you to control the aspect ratio of the boundary layer cells (or prism cells) that

are extruded from the base boundary zone.The aspect ratio is defined as the ratio of the prism base

length to the prism layer height.

smooth-transition: allows you to use the local tetrahedral element size to compute each local initial

height and total height so that the rate of volume change is smooth. Each triangle that is being in-

flated will have an initial height that is computed with respect to its area, averaged at the nodes.

This means that for a uniform mesh, the initial heights will be roughly the same, while for a varying

mesh, the initial heights will vary

uniform: allows you to generate every new node (child) to be initially the same distance away from

its parent node (that is, the corresponding node on the previous layer, from which the direction

vector is pointing).

last-ratio: allows you to control the aspect ratio of the boundary layer cells (or prism cells) that are

extruded from the base boundary zone.You can specify First Height for the first prism layer.

i.

If the Offset Method Type is set to smooth-transition or last-ratio, specify the Transition Ratio.

This value determines the ratio of the height of the last layer in the inflation and the first cell in

the volume fill.

ii.

If the Offset Method Type is set to aspect-ratio, specify the First Aspect Ratio.You can control

the heights of the inflation layers by defining the aspect ratio of the inflations that are extruded

from the inflation base.The aspect ratio is defined as the ratio of the local inflation base size to

the inflation layer height.The value for the First Aspect Ratio allows you to specify the first aspect

ratio to be used.

iii. If the Offset Method Type is set to uniform or last-ratio, specify the First Height.This value is

the height of the first layer of cells in the boundary layer.

iv. If the Offset Method Type is not set to last-ratio, provide the Growth Rate.This value determines

the relative thickness of adjacent inflation layers. As you move away from the face to which the

inflation control is applied, each successive layer is approximately one growth rate factor thicker

than the previous one.

b. Specify the Number of Layers.This value determines the maximum number of boundary layers to

be created in the mesh.

c.

Click Advanced Options to access additional controls prior to performing this task. See Improving

Prism Mesh Quality (p. ) for more information. Options include:

Use the Ignore Inflation at Acute Angles? option to choose whether to automatically ignore inflation

layers where there are acute angles.

Use the Inflation Gap Factor option to specify the relative gap between two boundary layer caps

in a narrow channel. A value of  indicates a gap that is of the same order as the boundary layer

cap triangle size in the inflation layer.

Use the Inflation Max Aspect Ratio option to specify the maximum aspect ratio for the inflation

layer when proximity compression is applied.

Use the Inflation Min Aspect Ratio option to specify the minimum aspect ratio for the inflation

layer.

Use the Keep First Inflation Layer Height option to retain the initial inflation layer's height.

Use the Adjacent Attach Angle option to set the angle for which the inflation would imprint on

an adjacent boundary.

. Provide volume settings.

a.

a.

Choose the type of Volume Fill that you require. Available options are:

tetrahedral

hexcore

polyhedra

poly-hexcore

b. Indicate whether to Mesh Solid Regions or not.This is enabled by default.

c.

If the Volume Fill method is set to tetrahedral or polyhedra, specify the Growth Rate.This value

determines the relative length-based size change of cells from the boundary (or the boundary layer

cap) towards the interior of the domain.

d. If the Volume Fill method is set to hexcore or poly-hexcore, specify the number of Buffer Layers

and Peel Layers.The buffer layers are additional layers of cells to alleviate an rapid transition from

finer cells to coarser cells (see Buffer Layers (p. ) for details).The peel layers are additional layers

that control the gap between the hexahedra core and the geometry (see Peel Layers (p. ) for details).

e. Use the Max Cell Length field to determine the maximum length of the volume mesh cell.

Note

Clicking in this field displays red boxes in the graphics window, providing a visual

representation of the field value. Use the Clear Preview button to hide the visualiz-

ation display.

f.

If the Volume Fill method is set to poly-hexcore or set to tetrahedral (with the Number of

Layers for the boundary layer is greater than ), the Enable Parallel Meshing option (enabled

by default) allows you to apply parallel processing of the volume mesh. The Enable Parallel

Meshing option is also only available when the number of parallel processors is greater than

). For information about parallel processing and automatically partitioning the mesh, see Auto

Partitioning (p. ). Disable this option if you are interested in only generating the volume

mesh in serial mode.

g. Click Advanced Options to access additional controls prior to performing this task. Options include:

Use the Invoke Persistent Renaming option to allow the volume mesh components to use

persistent and unique names for the solver. This will make zone names equivalent to region

names, and will make cell and face zone names unique. Using this field is highly recommended

for any parametric study.

Note

Persistent renaming only works if all body names are unique.

Use the Use Size Field? option to determine whether or not to use size fields as part of

generating the volume mesh.

Use the Polyhedral Mesh Feature Angle option to set the angle to preserve features when using

a polyhedral-based mesh.

Use the Avoid / Octree Transition? option to determine whether or not you want to avoid

any potential : cell transition in the hexcore region of the volume mesh, replacing any abrupt

change in the cell size with polyhedral cells.

Use the Fill Polyhedra in Solids? option to determine whether or not to apply polyhedral

cells to any solids during volume meshing.

Use the Quality Warning Limit option to the set the threshold for when mesh quality warnings

are generated.

. Click Create Volume Mesh to generate a volume mesh for the imported CAD geometry.

. Use the Draw Mesh button to display the fluid and/or solid meshes.

Figure . : Example of a Fluid and a Solid Volume Mesh

Additional enhancements can be made to the volume mesh using the Improve Volume Mesh task

(see Improving the Volume Mesh  (p. )). For more information about volume meshing, see Object-

Based Volume Meshing (p. ).

When you are satisfied with the volume mesh, you can proceed to setting up your CFD simulation in

Fluent solver mode.

You can update the properties of any defined boundary using the Update Boundaries task. This task

can be added to the workflow as many times as you require.

. Choose a Selection Type as either by label or by zone.

. (optional) Rename any Boundary Name by double-clicking the label in the table and entering a new

name.

You can also rename a boundary by selecting it in the table, right-click, and select Set Boundary

Name in the context menu, and provide a new name directly in the menu.

. (optional) Re-assign any Boundary Type to another value by selecting a type in the table and using the

corresponding drop-down menu. Choices include:

symmetry

wall

outflow

Multiple boundaries can be assigned a specific type all at once by selecting them in the table, right-

symmetry

wall

outflow

click, and select Set Boundary Type in the context menu, then designate a type for the selected

boundaries directly in the menu.

. (optional) By default, the table only lists external wall boundaries. Select the List All Boundaries

to see additional boundaries, such as fluid-fluid internal boundaries.

. When you are satisfied with the boundary assignments, click Update Boundaries.

. Use the Draw Boundaries button to visualize all boundaries or just wall boundaries.

Multiple boundaries can be visualized all at once by selecting them in the table, right-click, and

select Draw Selections in the context menu.

. Once all boundaries have been updated, proceed to the next step in the workflow.

Additional boundary types can be created using the Add Boundary Type task (see Adding Boundary

Types (p. )).

You can make improvements to your surface mesh using the Improve Surface Mesh task. For addi-

tional information, see Face Connectivity Issues (p. ) and Quality Checking (p. ).

. Provide a value for the Face Quality Limit.

Use the Quality Improve Max Angle option to set the maximum angle between the normals of adjacent

faces during mesh improvements.

Use the Quality Improve Iterations option to specify the number of iterations that will be performed

to improve the mesh.

Use the Quality Improve Collapse Skewness Limit option to specify the limiting skewness value when

improving the mesh. After quality improvements using the Quality Improve Max Angle are performed,

if any remaining triangles are above the Quality Improve Collapse Skewness Limit, these will be ag-

gressively removed using a fixed maximum angle of  degrees.

. Click Improve Surface Mesh.

Note

Changing the Face Quality Limit too extensively can result in aggressive changes to your

surface mesh.

You can create additional boundaries for your simulation using the Add Boundary Type task. This

task can be added to the workflow as many times as you require.

. Provide a Name for the new boundary, or use the default name. The default name changes depend-

ing on the assigned Boundary Type.

. Choose the Boundary Type. Choices include:

symmetry

wall

outflow

. Use the Zones list to select an available zone to apply to the boundary.

. Click Add Boundary Type.The new boundary will appear in the workflow.

You can make improvements to your volume mesh by using the Improve Volume Mesh task.

. Provide a value for the Cell Quality Limit.

Use the Quality Improve Min Angle option to set the minimum angle between the normals of adjacent

Use the Ignore Features for Remaining Bad Cells? option to choose whether or not to ignore prob-

lematic cells.

. Click Improve Volume Mesh.

For more information, see Improving the Mesh (p. ) or Improving Prism Mesh Quality (p. ).

You can perform additional enhancements to your surface mesh using the Modify Mesh Refinement

task. It is not recommended to use this task to coarsen the mesh locally, particularly on curved surfaces,

instead, perform any coarsening operations using the Add Local Sizing task (see Adding Local Siz-

ing (p. ) for more information).

. Provide a Name, or use the default name (soft_size_1).

. Choose a means for adding or controlling the remeshing using the Refinement Sequence drop-down

menu.

You can choose to simply Add a mesh refinement control, and remesh later when the task is

completed and updated, or you can choose to Add and Remesh a mesh refinement control that

will add the control and perform a remeshing operation at the same time.

When Add & Remesh is used, and you select only one label, no additional labels are created. In

all other cases, a new label is created, representing the selected zones/labels.

. Specify a Local Size.

. Choose a selection method using the Select By field.

Note

Use the Remesh Feature Min Angle option to specify the minimum angle for which features will be

preserved upon remeshing.

Use the Remesh Feature Max Angle option to specify the maximum angle for which features will be

Use the Remesh Corner Angle option to specify the corner angle for remeshing.

. Click Modify Mesh Refinement.The additional surface mesh settings will be applied and visible. For

more information about surface meshes, see Object-Based Surface Meshing (p. ).

Customize your meshing workflow using the Run Custom Journal task.

Use a text editor to copy portions of any of your own journal files, and paste them into this task to

perform additional meshing refinement. See Customizing Workflows (p. ) for more information.

Once you are satisfied with your changes, click Run Custom Journal, and proceed to the next step in

the workflow.

Note

This task can be added to the workflow as many times as you require, however, this task

cannot be the initial task in a custom workflow. In addition, this task assumes that you are

familiar with scripting and the available standard Fluent commands in meshing mode. See

Query and Utility Functions in the Fluent Text Command List - Wrap Functions in the Fluent

Text Command List for more information.

This section describes the various tasks that are provided when using the Fault-tolerant Meshing

guided workflow:

... Importing CAD Geometries and Managing CAD Parts

... Describing the Geometry and the Flow

... Creating External Flow Boundaries

... Creating Local Refinement Regions

... Identifying Construction Surfaces

... Extracting Edge Features

... Adding Thickness to Your Geometry

... Creating Porous Regions

... Identifying Regions

... Defining Leakage Thresholds

... Updating Your Region Settings

... Choosing Mesh Control Options

... Setting Up Size Controls

... Generating the Surface Mesh

... Setting Up Boundary Layer Controls

... Generating the Volume Mesh

... Separating Contacts

Use the Import CAD and Part Management task to import one or more CAD files into your simulation

and to perform selective management of which parts you may want to include in your simulation, if

needed. Selected parts are then designated as potential meshing objects, where selective settings can

be adjusted as desired. Upon completing the task, meshing objects are created for later use in your

Fluent simulation.

You can import one or more CAD geometry files into your workflow, as well as append additional files

as needed. Once specified, you can determine how the portions of your CAD geometry will be converted

into meshing objects for your simulation: automatically by part, or by manually choosing your custom

parts or assemblies.

Upon loading the CAD geometry, you can view the components of the CAD geometry in the CAD

Model tree. You can also view potential meshing objects in the Meshing Model tree. Various properties

for your meshing objects (such as feature extraction angle, or custom refaceting settings) can be viewed

and adjusted accordingly. When you are satisfied with your meshing model objects and their properties,

you can complete the task, thereby creating meshing objects for later use in your Fluent simulation.

. For the CAD File field, provide a path and a name for the CAD file that you want to load into the task, or

use the (…) button to browse for a specific file.

Standard ANSYS file types are supported, including .scdoc, .agdb, .fmd, .fmdb, .fmd, .pmdb,

.tgf, and .msh.

Other CAD formats are also supported, including .jt, .plmxml, .stl, .CATPart, .CATProduct,

.prt, .x_t, .sat, .step, .iges, and.igs. See, for example, File Format Support for additional

formats.

. Select an appropriate Import Route option, or keep the default value, depending on your require-

ments and platform. In most cases, the default value is recommended and should lead to the desired

data being imported, however, you should be aware of and verify the CAD configurations being

made because they may be considered during import. See CAD Integration for details.

The workflow uses an .fmd file to extract and persist CAD information for this task. To generate

an appropriate .fmd file, the available options for the Import Route depend on the selected CAD

File, and your particular platform (Windows or Linux). The various Import Route options include:

The Native option loads the CAD file natively into FM, and internally generates an FMD file that is then

loaded into the workflow.This option is available for .fmd, .fmdb, and .stl file formats.

Note

Using this import route, the CAD data should not differ across Windows and Linux

for default settings.

Note

Using the Fault-tolerant Meshing Workflow

The SCDM option uses ANSYS SpaceClaim Direct Modeler to read the CAD file and internally generates

an .fmd file that is then loaded into the workflow.You may also want to note any SpaceClaim file options

that you may have configured.

Note

This route is only available on Windows, and is not available on Linux.

The Workbench option uses ANSYS Workbench CAD readers or plug-ins to attach or load the given

CAD file and generates an .fmd file that is then loaded into the workflow.

Note

This route is available on Windows and Linux., though not all formats are supported

on Linux when compared to Windows. Also, third-party add-on modules can lead to

slightly different CAD data upon import (for example, names, assembly hierarchy,

etc. ).

The ACIS option is the default import route for .sab and .sat file types.

The MSH option is the default import route for .tgf and .msh file types.

The JTOpen option is the default import route for .jt  and .plmxml file types, and only faceted

data is imported.

Note

The JTOpen option is available on more recent Linux OS variants (requiring a glibc

supplying 'memcpy@GLIBC_2. '), that is, it is not supported on Red Hat / CentOS

series.

. For selected .stl files, use the File Unit field to indicate the units in which the file was created.

Note

Imported .stl files can have different sets of units.

. For selected .jt files using the JTOPEN import route, you can use the Jt LOD field to choose the

level of CAD tessellation accuracy (level of detail) exposed after import. For example, typically, you

might have three levels of detail (such as,  for 'fine',  for 'medium', and  for 'coarse') but up to

ten might be contained in the .jt file. If a certain level of detail does not exist in the file, the next

finer level of detail is taken automatically.

. Select an option from the Create Meshing Object Per field.

Choose One per part so that Fluent automatically creates meshing objects for all the parts within the

CAD model.

Choose Custom to be able to manually assign which parts of your CAD model are to be included as

meshing objects in your simulation.

. Use the Display Unit field to specify the units that you want to work with when the geometry and mesh

is displayed in the graphics window.This field also specifies the dimensions of the generated mesh.

. Use the Load button to load the CAD file into the task.

Note

You can append additional CAD file(s) to your currently loaded CAD file. See Appending

CAD Files (p. ) for details.

. Use the CAD Model tree to visualize the hierarchy of your CAD model. By default, the CAD Model tree is

automatically populated with the components of the imported and/or appended CAD file(s). For more

information, see Working with the CAD Model Tree (p. )

. Use the Meshing Model tree to visualize the hierarchy of your meshing objects.

If Create Meshing Objects Per is set to One per part, the Meshing Model tree is automatically populated

with all of the corresponding parts from the CAD model, providing you with a preview of the number

of meshing objects that will be generated.

If Create Meshing Objects Per is set to Custom, the Meshing Model tree is initially empty, and you

can select individual parts and manually add them to the Meshing Model tree, providing you with a

more customized approach to the number of meshing objects that will be generated.

For more information, see Working with the Meshing Model Tree (p. ).

. Set various properties, such as feature extraction angle, or custom refaceting settings, for selected

meshing objects (

). See Setting Properties for Meshing Model Objects (p. ) for details.

. Once your selections are made, click Create Meshing Objects to generate a collection of meshing objects

based on the imported CAD geometry.

.... Appending CAD Files

Once a CAD file is loaded into the Import CAD and Part Management task, you can append addi-

tional files to the current CAD model.

a.

Select the Append checkbox.

b. Specify additional CAD files in the Append File field, provide a path and a name for the CAD file

that you want to import, or use the (…) button to browse for a specific file.

c.

For selected .stl files, use the File Unit field to indicate the units in which the file was created.

Note

Appended .stl files can have different sets of units.

d. For selected .jt files using the JTOPEN import route, you can use the Jt LOD field to choose

the level of CAD tessellation accuracy (level of detail) exposed after import.

e. Repeat as required, and when finished, select the Append button.

The contents of the appended file(s) are added to the tree, after the original CAD objects

....Working with the CAD Model Tree

Many CAD models contain tens and hundreds of separate components, and you might only be inter-

ested in performing a CFD simulation on a small portion of those components. In the CAD Model

tree, you can take portions of the CAD model and isolate them for your simulation by moving them

from the CAD Model tree and placing them into the Meshing Model tree.

Figure . : A CAD File Loaded into the CAD Model Tree

Objects in the CAD Model tree can be assemblies (

) or parts (

).You can have any number of levels

in the tree.

Select CAD model objects directly in the tree in order to perform various tasks. Use Ctrl+left-click to select

multiple non-sequential objects in the tree. Use Shift+left-click to select multiple sequential objects in

the tree. See Using Hot Key Shortcuts in the Model Trees and the Graphics Window (p. ) for additional

selection and display shortcuts for this task.

Note

An object is highlighted when it is selected in the tree. The checkbox for an object is

used for displaying that object in the graphics window.

Alternatively, you can right-click the object directly in the graphics window, and it will become

selected in the corresponding tree. Use Ctrl+right-click to select multiple objects in the graphics

window (and thereby selecting multiple objects in the tree).

Display a CAD model object in the graphics window by enabling the checkbox (

) to the left of object

in the tree. Likewise, to hide an object from view in the graphics window, disable the checkbox. Select-

ing/deselecting a parent assembly node in the tree to show/hide the geometry in the graphics window

allows for all of its component parts to also be shown/hidden.

Use the Filter Text field to perform name-based searching and filtering on models containing a

large number of components.

Select and move objects from the CAD Model tree and place them in the Meshing Model tree:

– Drag and drop components from the CAD Model tree onto the Meshing Model tree on the right.

– Alternatively, identify one or more part(s) - by enabling the corresponding checkbox(es) - in the CAD

Model tree, right-click and select Move Checked to Active Node in the context menu, so that all of

the graphically visible objects are moved to active node

– Select the object(s) directly in the graphics window, and use the Ctrl+middle-click mouse button

combination to move them from the CAD Model tree to the Meshing Model tree.

Selecting an object directly in the graphics window also selects the corresponding object in the

tree. You need to right-click on an object to select it in the graphics window. Use Ctrl+right-

click to select multiple objects in the graphics window, thereby selecting the corresponding

objects in the tree.

– As items are moved from the CAD Model tree, they become grayed out in the CAD Model tree and visible

in the Meshing Model tree. If you mistakenly add a component to the Meshing Model tree, you can

easily remove it using the Restore to Cad Model option from the context menu, thereby adding it back

to the CAD Model tree.

If the CAD Model tree is active, you can visualize the checked CAD objects by clicking the Show CAD

Model button.

Various features are available from the context menu of the CAD Model tree, depending on what is selected,

including:

– Use the Move Checked to Active Node option to automatically move the checked object to the active

node in the Meshing Model tree.

– Use the Create Meshing Object for Each Part option to automatically create a part for the selected

object and move it to the Meshing Model tree.

– Use the Hide Others option to display only the selected items in the graphics window.

....Working with the Meshing Model Tree

The Meshing Model tree is primarily populated with selective parts from your CAD model. The com-

ponents in the Meshing Model tree will be the pieces of your CAD model that you want to include

in your Fluent simulation. They will ultimately become meshing objects, and visible as such, in the

Outline View in your Fluent session.

Figure . : Selected Portions of a CAD File Loaded into the Meshing Model Tree

Objects in the Meshing Model tree can be top-level meshing objects (

) or parts (

).You can only

have two levels in the tree.

Select meshing objects directly in the tree in order to perform various tasks. Use Ctrl+left-click to select

Note

window, thereby selecting multiple objects in the tree.

Display a meshing object in the graphics window by enabling the checkbox (

) to the left of object in

the tree. Likewise, to hide an object from view in the graphics window, disable the checkbox. Select-

Set various properties for selected meshing objects (

). See Setting Properties for Meshing Model Ob-

jects (p. ) for details.

If the Meshing Model tree is active, you can visualize the checked meshing objects by using the Show

Meshing Model button at the bottom of the task.

Various features are available from the context menu of the Meshing Model tree, depending on where in

the hierarchy you are located, including:

– Use the Create Object option to add a generic object to the tree.

By default the Meshing Model tree is empty, however, using the Create Object option from the

context menu, you can create your own custom collection of object categories, where you can

add components from the CAD Model tree. Once created, you can save that collection of simu-

lation meshing objects using the Save Meshing Objects icon (

) where you can save the

object collection in a .mmt file. If you need to use that collection of objects again, you can use

the Load Meshing Objects icon (

) and locate a previously saved .mmt file.

The *.mmt object collection files include the version number of the current release (for example,

for the  R3, release, the files are internally designated with "version": ". ".

You can also use the Select a template drop down field above the tree to choose an available

template of objects, such as External Flow, which contains a template of object categories

specific to typical external flow objects.

– Use the Rename option to assign a new name for the selected object in the tree.

– Use the Set as Active Node option to specify the current node as the active node.The active node's

label is indicated in bold.When a node is selected as the active node, you are able to transfer checked

CAD model objects more easily to the active node using the context menu.

– Use the Restore to Cad Model option to remove the selected item from the tree and restore it in the

CAD Model tree.

.... Setting Properties for Meshing Model Objects

Meshing model objects listed in the tree have various properties that you can set, if necessary. For

custom meshing object creation (that is, when you have set the Create Meshing Object Per field to

Custom), these properties are available under Advanced Object Settings.

Figure . : Properties of a Selected Custom Meshing Model Object

Set the Create One Zone Per option to object, part, body, or face, accordingly. For instance, if face

is selected, each CAD surface or face will be assigned to a face zone.

Specify a value for the Feature Extraction Angle field, or use the default value of  degrees, to

specify the angle at which features will be extracted from the CAD model on import. See Faceting

Considerations (p. ) for details.

Enable or disable the Prefix Object Name to Zone Name accordingly. Enabling this allows for

naming the corresponding face zone using the object name as a prefix.This option is available only

for custom meshing object creation.

When creating meshing objects by part, use the Refacet checkbox to enable or disable additional

faceting refinement in this task.When enabled, you can change the faceting of the selected object.

Likewise, for custom meshing object creation, use the Refacet During Update checkbox to enable

or disable additional faceting refinement when this task is updated. Refaceting will refacet the original

CAD geometry. Only the faceted CAD model is used during the meshing process. In either case, when

disabled, normal CAD faceting is performed as defined by the imported CAD file(s).

– The Deviation controls how far facet edges are away from the model.

– The Normal Angle also controls how far facet edges are away from the model. Decreasing the

normal angle will result in more facets along the curved edges.

– The Max Size controls the maximum size of the facets after the deviation and the normal angle

are respected.

In the following example, the left-hand model uses small values for the deviation and the

normal angle in order to capture the curved surface, and a large value for the maximum size

in order to get larger facets on the flat surface. The right-hand model uses larger values for

the deviation and the normal angle in order to capture the curved surface coarsely, and a

smaller value for the maximum size in order to capture the flat surface evenly.

For custom meshing object creation, you can:

– When refaceting is enabled, use the Preview Refacet button to preview changes to

the refaceting settings in the graphics window while you are still within the task. Change

values and repeat as needed for as many objects in the tree as required.

– Use the Copy Settings to Child Objects button to apply changes to these properties to

any child objects associated with the selected parent object in the tree.

– Use the … menu button at the bottom of the task, and select the Save FMD option to save

your changes in a new .fmd file for future use. This is especially useful for particularly large,

complicated models in which you have made many specialized changes to the properties

(such as refaceting), and allows for a faster load time. Note that mirrored components cannot

be saved to the .fmd format.

..... Faceting Considerations

Faceting is very important for many reasons: if the faceting is too coarse, you will lose fidelity; if the

faceting is too fine, then you will not capture important features in rounds or fillets.

Figure . : Faceting Example

Here the minimum facet edge in the fillet is roughly the same size as the minimum local size control

to be used. Once feature edges are extracted using  degrees, you will have:

This will lead to faster graphics operation (due to lighter model), faster meshing, and better feature

capturing. Even if the target size becomes larger (not more than  times), it will still respect those

feature lines, leading to anisotropic mesh, and reduced cell count.

.... Setting Display Options for CAD Model and Meshing Objects

To change how different components are colored and displayed in the graphics window, use the …

menu button at the bottom of the task, and select Display Options.

This displays the Display Options dialog:

The Display Options dialog allow you to select color preferences for the displayed components of

the CAD Model tree or the Meshing Model tree. Options include to color by Default (automatic), by

CAD, by Component, or by Objects. You can also provide an Area Selection Tolerance.

.... Using Hot Key Shortcuts in the Model Trees and the Graphics Window

In addition to the hot key shortcuts that are available in Fluent in meshing mode (Appendix C: Shortcut

Keys (p. )), the following selection and display hot key shortcuts are available in the Import CAD

and Part Management task:

Keys

Action

Ctrl+I

Keys

Action

Ctrl+I

Select component instances

Selection

Tools

Ctrl+P

Select parent assembly

f2

Clear selections

Ctrl+Y

Clear CAD Model tree selections

Ctrl+J

Preview the other display mode

Display

Mode Tools

Ctrl+K

Disable the preview of the other display mode

Ctrl+L

Toggle between the preview of the other display mode

Keys

Action

Ctrl+Shift+A

Show all

Display

Tools

Ctrl+Shift+E

Show/hide edges

Ctrl+Shift+H

Hide

Ctrl+Shift+I

Isolate

Ctrl+D

Miscellaneous Compute distance

Tools

Ctrl+H

Print this help

Ctrl+X

Position filter

f3

Toggle right mouse button

f4

Toggle selection method

Ctrl+A

Auto scale

Ctrl+B

CAD object filter

The Describe Geometry and Flow task lets you specify the type of geometry you have and the type

of flow you are trying to simulate. Settings in this task determine what sub-tasks are available for the

overall task.

. For the Flow Type, choose from the following:

If you are going to be simulating external flow over or around an object (such as a truck, car, bicycle,

etc. ), select External flow around object and a Create External Flow Boundaries task is added

to the workflow (see Creating External Flow Boundaries (p. )).

If you are going to be simulating flow within an object (such as a manifold, or catalytic converter,

etc. ), select Internal flow through the object and an Enclose Fluid Regions (Capping) task is

added to the workflow (see Enclosing Fluid Regions (p. )).

. For external flows, indicate whether or not you will require any enclosures to capture external flow

regions. If you select Yes, then a Create External Flow Boundaries task is added to the workflow

(see Creating External Flow Boundaries (p. )).

. Indicate whether or not your geometry will require any local refinement regions. If you select Yes,

then a Create Local Refinement Regions task is added to the workflow (see Creating Local Refinement

Regions (p. )).

. Indicate whether or not your geometry contains any predefined construction surfaces (such as cylinders

for moving reference frames, or capping surfaces, etc.). If you select Yes, then an Identify Construction

Surface task is added to the workflow (see Identifying Construction Surfaces (p. )).

Indicate whether or not your geometry contains any zones with zero thickness. If you select Yes,

then an Add Thickness task is added to the workflow (see Adding Thickness to Your Geo-

metry (p. )).

Indicate whether or not your geometry will require any form of edge or feature extraction. If you

select Yes, then an Extract Edge Features task is added to the workflow (see Extracting Edge

Features (p. )).

Indicate whether or not your geometry contains any porous regions. If you select Yes, then a

Create Porous Regions task is added to the workflow (see Creating Porous Regions (p. )).

. Once your selections are made, click Describe Geometry and Flow and proceed onto the next task.

For internal flow simulations with solid model geometries, you can use the Enclose Fluid Regions

(Capping) task to cover, or cap, any openings in your geometry in order to later calculate your fluid

region(s).

. Specify a Name for the capping surface.

outflow

symmetry

wall

available zones in the list before selecting a zone.You are able to select multiple zones for capping.

Note

When simulating external flow around an object, your geometry may not contain a fully defined ex-

ternal flow boundary. You can manually create an external flow boundary in this task, by defining a

bounding box that surrounds the relevant aspects of your geometry, such as around a vehicle.

Figure . : An Example of an External Flow Boundary

. Specify a Name for the external boundary, or use the default name (tunnel).

. For Method, select Create a new external flow boundary if you are creating a new external boundary,

or select My geometry already has an external flow boundary if the external boundary is already

defined as part of your imported geometry.

. Choose whether to Select By the object name or the zone name in the list below.

If you Select By object, in the Objects list, you can choose an object in the list, or enter text to filter

out the available objects in the list before selecting an object.

. Once one or more object(s) or zone(s) is selected, you can define the extents of the external boundaries

around the selection by defining a bounding box.

. For new external flow regions, additional settings are required.

When you select Ratio relative to geometry size, the Box Parameters hold the minimum and

maximum extension ratios for the X, Y, and Z dimensions. By default, they are set to extend the

dimensions of a bounding box around your selected object(s) or zone(s) out by a factor equivalent

to the total singular length of the geometry in the X, Y, and Z directions. You can change the values

according to your needs, and the display in the graphics window will change accordingly.

When you select Directly specify coordinates, the Box Parameters hold the minimum and max-

imum extension distance for the X, Y, and Z dimensions. By default, they are set to values that

correspond to the extension ratios, but you can set them to more suitable values as required, and

the display in the graphics window will change accordingly.

Figure . : An External Flow Bounding Box

. Once your selections are made, click Create External Flow Boundaries and proceed onto the next task.

Figure . : An External Flow Boundary Around a Car

When simulating flow within and around an object, your geometry may not contain a fully defined

refinement region, or body of influence (BOI). If a volume region needs mesh refinement, that region

can be identified by watertight surface. You can manually create such a surface in this task by: defining

a bounding box around one or more selected objects; using one or more existing objects that have

already been imported; or creating an offset surface. For example, this volume region, which surrounds

the relevant aspects of your flow physics, can be used to as an alternative to refine the mesh in a

particular area, such as the wake region behind a vehicle.

Figure . : An Example of a Refinement Region Around a Car

. For Type, choose from the following:

Select Box to define a bounding box for the refinement region.

Select Existing if the refinement region is already defined as part of your imported geometry.

Select Offset Surface if the refinement region will be offset from the surface of an existing object or

zone that you will select.

. Specify a Name for the body of influence, or use the default name (local-refinement-).

. Specify a value for the Min Size for the refinement region.

. Once one or more object(s) or zone(s) is selected, you can define the extents of the refinement region

. Depending on the Type of refinement region, additional parameters are required.

For a Box refinement region:

– When you select Ratio relative to geometry size, the Box Parameters hold the minimum and

maximum extension ratios for the X,Y, and Z dimensions. By default, they are set to extend the di-

mensions of a bounding box around your selected object(s) or zone(s) out by a factor equivalent to

the total singular length of the geometry in the X,Y, and Z directions.You can change the values

– When you select Directly specify coordinates, the Box Parameters hold the minimum and maximum

extension distance for the X,Y, and Z dimensions. By default, they are set to values that correspond

to the extension ratios, but you can set them to more suitable values as required, and the display in

the graphics window will change accordingly.

For an Offset Surface refinement region:

– Specify the Flow Direction. It is used to determine the wake.The wake is downstream of the selected

geometry object(s).

– Use the Flip option if the flow direction is in opposite direction.

– Specify a value for the Defeaturing Size, or use the default value.This will obtain the rough shape

of the selected object(s), which are wrapped using this size.

– Specify a value for the Total Boundary Layer Height, or use the default value.This how far from the

selected object (s) the rough shape is offset.

– Specify a value for the Boundary Layer Levels, or use the default value, to determine the number

of offset surfaces to be created.

– Specify a value for the Wake Growth Levels, or use the default value.The rough shape is scaled in

the wake direction as well as in the cross-wake direction.This value determines how many scaled

offsets are to be created.

– Specify a value for the Wake Growth Factor, or use the default value. Each scaled offset surface is

grown in size in the wake direction by this factor from the previous scaled offset.

– Specify a value for the Cross Wake Growth Factor, or use the default value. Each scaled offset surface

is grown in size in the cross-wake direction by this factor from the previous scaled offset.

For example, given an automobile geometry, the base is the surface on the vehicle, which has

maximum size of  mm. The following size control settings were automatically generated:

Max

Size

Size

Function

Name

soft

name

boi

name-

boi

name-

boi

name-wake-

boi

boi

boi

Max

Size

Size

Function

Name

soft

name

boi

name-

boi

name-

boi

boi

boi

boi

The refinement regions and the various settings can be visualized using Figure . : An Example

of Multiple Refinement Regions Around a Car (p. ) and Figure . : An Example of Multiple

Refinement Regions Around a Vehicle (p. ).

Figure . : An Example of Multiple Refinement Regions Around a Car

Figure . : An Example of Multiple Refinement Regions Around a Vehicle

. Once your selections are made, click Create Local Refinement Regions and proceed onto the next task.

For more information about bodies of influence, see Body of Influence (p. ).

For geometries that have primitive construction surfaces (e.g., capping surfaces, or cylindrical surfaces

for moving reference frames) already defined as part of the CAD model, you can use the Identify

Construction Surface task to locate those portions of the geometry and identify them as such so that

Fluent can handle them accordingly during the meshing process. These surfaces are used to further

decompose the main fluid into multiple regions, such as regions around a rotating fan for a moving

reference frame (MRF) simulation.

. Specify a Name for the construction surface, or use the default name (construction-surface-).

. Choose an object in the list, or enter text to filter out the available objects in the list before selecting an

object.

object.

. Once your selections are made, click Identify Construction Surfaces and proceed onto the next task.

You can use the Extract Edge Features task to identify important geometric features in order to retain

their fidelity for your simulation and to improve the integrity of the final surface mesh. Once these

important feature are identified, additional operations are applied to imprint them onto the final surface

mesh. Size controls can also be applied to them to refine the mesh on those features.

. Specify a Name for the specific edge feature object, or use the default name (edge-group-).

. For the Extraction Method Using field, select the technique to be used for the feature extraction. Choices

are Feature Angle, Intersection Loops, or Sharp Angle.

. In the Objects list, you can choose an object in the list, or enter text to filter out the available objects in

the list before selecting an object.

. Depending on the extraction method, you will have to provide the following:

For the Feature Angle extraction method, specify the Feature Angle that you want to use as the

threshold for feature extraction. If the angle between two adjacent geometry facet normals is more

than this feature angle value, then a feature is extracted at the sharing edge.

For the Intersection Loops extraction method, specify the Intersected By option that you want to use

as the threshold for feature extraction: either individually or collectively.This is a feature located at

the intersection of two geometry facets. For collectively, only facets across objects are considered. For

individually, all facets are considered.

For the Sharp Angle extraction method, specify the Sharp Angle that you want to use as the threshold

for feature extraction. If the angle between two adjacent geometry facet normals is more than this

sharp angle value, then a feature is extracted at the sharing edge.The default angle is  degrees, in-

dicating that these surfaces have a very sharp angle between them.You can define more refined size

controls on them and also apply special operations on these objects to force sharing nodes of the final

surface mesh onto the geometry.

Figure . : An Example of Addressing Sharp Angles - CAD Geometry

Figure . : An Example of Addressing Sharp Angles - Final Mesh

Figure . : Sharp Angles With and Without the Zones Separated By Face

To force the sharing nodes, the geometry face zones need to be separated at the sharp angle

edge. Select face zones per part for that object.

. Once your selections are made, click Extract Edge Features and proceed onto the next task.

Some portions of an imported geometry may not have a thickness (such as a baffle, or other interior

wall, for instance), and may be important or relevant to your simulation. A more refined surface mesh

can be generated if all important and relevant aspects of the geometry have a certain thickness. Not

all portions of a geometry require a thickness. However, if it has no thickness, and is important for

your simulation, and contains an adequate number of quality geometry facets, then you can use the

Add Thickness task to define a thickness to that portion of the geometry. The geometry is thickened

in the normal direction of the facets. You may want to reverse the facet normal direction (see Manip-

ulating Boundary Zones (p. )) before applying this operation.

. Specify a Name for the zero thickness geometry, or use the default name (face_group).

. Specify the Offset Distance that you want to use as the distance for the zero thickness geometry.The

geometry will be thickened by this value.

. Once your selections are made, click Add Thickness and proceed onto the next task.

The following illustrations demonstrate some examples of requiring thickness:

If your geometry contains some regions where porous media is present and you need to simulate flow

through those porous regions, you can use the Create Porous Regions task to define portions of your

geometry that will exhibit porous behavior in the flow field.

Figure . : An Example of a Porous Region

Figure . : An Example of a Porous Region: Fins and Tubes in a Heat Exchanger

Simulating the pressure drop of the fluid passing through a porous media requires a separate region.

This separate porous region requires a very course and structured mesh. The Create Porous Regions

task can be used to generate such a mesh, which is used for rectangular-shaped regions.

. Specify a Name for the porous region, or use the default name (porous-region).

. Choose whether the Specify location by field is set to Node Selection or Position Selection.

. Use the right mouse button to select four points in the graphics window to define the porous region (P1,

P2, P3, and P4).Their coordinates will be listed in the table in the task.

Figure . : The Points of a Porous Region

. Specify a value either for the Cell Size Between P1 and P2 or the Number of Cells.

. Specify a value either for the Cell Size Between P1 and P3 or the Number of Cells.

. Specify a value either for the Cell Size Between P1 and P4 or the Number of Cells.

. Specify a value for the Buffer Size Ratio along with the Buffer Size.There are two advantages for having

a buffer zone:

The wrapper will not detect the inlet or outlet of the core, which will avoid zone recovery issues, making

for a much cleaner rezoning of the wrapper surfaces.

The macro-based heat exchanger model in the Fluent solver does not allow mesh interfaces at the in-

let/outlet of the core.With the buffer layer, the inlet and outlet are conformal, and the buffer can be

very thin (for example,  to  mm).

Figure . : The Buffer Size for a Porous Region

. Once your selections are made, click Create Porous Region and proceed onto the next task.The final

cell zone for the porous region will be created. Fluent will also create a geometry object for all triangulated

bounding faces.

In complex geometries, there could be hundreds or thousands of regions ranging in various sizes,

however, much of the time, you are only interested in only a few regions. Use the Identify Regions

task to pinpoint specific regions in your imported geometry, such as a vehicle in an external flow

simulation. Here, you are positioning specific points in the domain where certain objects of interest

can be identified and classified for later use in your simulation.

In most cases, there is not a single object that defines a region. Such regions, such as most fluids and

some voids, can only be identified using a specific point (also referred to as a material point).

Figure . : Identifying a Fluid Region in the Wake Behind a Car

Note

Material points can also be placed inside any additional regions that will be created as a

result of the decomposition of the main fluid region by construction surfaces (see Identifying

Construction Surfaces (p. )). If material points are not placed inside any of the decomposed

regions, these regions will be automatically identified and named according to the name

of the construction surface. For example, if you have identified a construction surface in

your workflow, named fan_mrf, any decomposed regions created from this construction

surface and which neighbors any user-defined regions, will be automatically named as

fan_mrf-, fan_mrf-, etc.

For the Would you like to identify any fluid or void region(s)? field, keep the default value of yes

if your model requires you to specify any fluid or void regions using the following steps. Otherwise,

select no, click Update and proceed to the next task.

. Specify a Name for the region, or use the default name (fluid-region-).The default name changes

depending on the assigned Region Type.

. For Define Location Using, select Centroid of Objects to calculate the position of the region based on

the centroid of the selected object(s), or select Numerical Inputs to assign specific coordinates to a par-

ticular region.

. Choose a Region Type for the region (either fluid or void).

. For the Link to Construction Surface(s) field, keep the default value of no for most cases involving a

singular fluid region. If, however, you mean to identify an additional fluid region that is either inside or

adjacent to a construction surfaces, then set this value to yes in order to properly mesh the additional

fluid region accordingly (that is, using a surface mesh).

. Use the View Exact Coordinates field to see the specific coordinate values for the region's identified

location.

. Once your selections are made, click Identify Regions and proceed onto the next task.

Note

If you have previously defined regions based on specific meshing objects that you sub-

sequently remove or rename (for example, in the Import CAD and Part Management

task), you may need to revert this task in order to refresh the list of meshing objects

available for your region definition. Fluent will prompt you if the list needs to be re-

freshed.

Once you have defined all of your objects in the Import Geometry and Part Management task, it's

freshed.

always recommended to make sure that there are no large parts missing and that all the parts fit to-

gether well. For instance, an imported car geometry may be missing a large part (such as a door),

resulting in a large hole and causing potential flow leakage into the cabin. There may also be potential

imperfections in the geometry (for example, missing bolts, missing sealants, etc. ), resulting in other,

medium sized holes. These holes may be larger than any of your initial local size controls, resulting in

leaks that need to be closed.

Any missing, misaligned parts, or small imperfections will lead to leakages that need to be identified

and closed using this task.

For the Would you like to close any leakages for your region(s)? field, select yes if your model re-

quires you to locate and address any leakage issues using the following steps. Otherwise, if your

model does not have any leakage issues to address, keep the default of no, click Update and proceed

to the next task.

. Specify a Name for the leakage threshold control, or use the default name (leakage-).

. Use the Regions list to select the region that requires a leakage threshold control.

. Specify a Maximum Leakage Size.

. Select the Preview Leakages button to see if there are any leakages present or not. If you can see leakages

occurring between regions, adjust the Maximum Leakage Size and click the Preview Leakages button

again to reconstruct the generalized mesh. Repeat as needed until all leaks have been resolved.

Figure . : Identifying Potential Leakages Within a Car

. Use a Leakage Plane controls to assess the interior of your geometry to help you to preview and identify

leakages.

Use the slider to adjust the Location accordingly to visualize any leakages.

Specify the Orientation as either in the X, Y, or Z direction.

Use the Flip option to flip the orientation of the clipping plane to suit your requirements.

. Once your selections are made, click Define Leakage Threshold and proceed onto the next task.

You can review and update the properties of any defined regions using the Update Region Settings

task. Any automatically detected regions will be filled with tetrahedral cells, designated as fluid, and

given a single layer of prism cells for the boundary layer.

. The Main Fluid field indicates the name of the primary fluid region for your simulation.

. Use the Displayed Regions field to indicate how your regions will be displayed in the table. You

can select All Regions, Object Based Regions, or Identified Regions. This can be helpful when

you have a large number of regions.

. Rename any region Name by double-clicking the label in the table and entering a new name.

. Choose a region Type as either fluid, solid, or void.

click, and select Set Type in the context menu, then designate a type for the selected regions directly

in the menu.

. Assign the Extraction Method to either wrap or surface mesh.

Multiple regions can be assigned a specific extraction method all at once by selecting them in the

table, right-click, and select Set Extraction Method in the context menu, then designate an extrac-

tion method for the selected regions directly in the menu.

Fluid regions that are within or adjacent to construction surfaces (using the Link to Construction

Surface(s) field) will automatically use the surface mesh extraction method.

. Choose a Volume Fill as either none, tet, or hexcore, or keep the default setting.

Multiple regions can be assigned a specific volume fill type all at once by selecting them in the

table, right-click, and select Set Volume Fill in the context menu, then designate a volume fill type

for the selected regions directly in the menu.

The options available for Volume Fill depend upon the selected Type(s). For a selected fluid region,

for example, you can only choose from tet or hexcore for the Volume Fill option. However, if you

select multiple regions, such as a fluid and a solid region, no options are available since there are

no volume fill types that can be applied to both region types.

. Specify a value for the Leakage Size, or keep the default value.

Multiple regions can be assigned a specific leakage size value all at once by selecting them in the

table, right-click, and select Set Leakage Size in the context menu, then specify a value for the

selected regions directly in the menu.

. When you are satisfied with the region assignments, click Update Region Settings.

. One or more regions can be visualized all at once by selecting them in the table, right-click, and select

The Choose Mesh Control Options task allows you to pick and choose various means of generating

and refining the mesh in your simulation.

. Specify how you would like to manage your size controls.

Select Create New to start with a new collection of size controls.

Select Read existing size control file to add your size controls based on those already defined in a

size control file (*.szcontrol), specified using the Size Control File field.

. If you are creating new size controls, you need to specify the nature of the size controls you are going to

use.

Select Default to populate your size controls with default settings, based on the number of objects in

your model. Using this option and updating the task will add a Setup Size Controls task to the workflow,

along with as many size controls as there are objects, each using the same default settings.

Select Custom to populate as many size controls as you need using your own customized settings.

Using this option and updating the task will add a single Setup Size Controls task to your workflow,

where you create as many size controls as you require.

For more information, see (see Setting Up Size Controls (p. ))

For the Apply quick edge proximity? prompt, select Yes to speed up the calculation and reduce

memory requirements when using a proximity size function with geometries having a very large

number of small feature edges.

Specify a value for the Solid/Fluid Size Ratio field, or keep the default. This is the ratio of the

actual size of the solid and the actual size of the fluid, used for solid meshing. For example, if

this ratio is . and the fluid size is , then the solid size will be ..

Specify a value for the Wrap/Target Size Ratio field, or keep the default.This is the ratio of the initial

wrap size and the local target size. For example, if this ratio is . and the target size is , then the

initial wrap size will be ..

. Once your selections are made, click Choose Mesh Control Options and proceed onto the next task.

Use the Setup Size Controls task to create individual sizing controls for your mesh. For every size

control that you create, it is added to the workflow as a subtask of the Setup Size Controls task.

. Specify a Name for the mesh sizing control, or use the default name (size-control-).

. Choose an option for the Size Functions field. Available options are:

Choose the curvature size function that computes edge and face sizes using their size and normal

angle parameters.

Choose the proximity size function that computes edge and face sizes in ‘gaps’ using the specified

minimum number of element layers.

Choose the soft size function that enables you to set the maximum size on the selected zone, while

the specified growth rate from the defined size influences the size on adjacent zones.

Choose the boi size function enables you to specify a body of influence (that is, a refinement region

for the sizing control).

. Specify a value for the Minimum Size for the size control when using the curvature or proximity size

function types.

. Specify a value for the Maximum Size for the size control.

. Specify a value for the Growth Rate for the size control.

. Specify a value for the Cells Per Gap when using the proximity size function type. Note that for proximity

size functions, the number of cells per gap can be a real value, with a minimum value of .. See Proxim-

ity (p. ) for more information.

. Specify a value for the Curvature Normal Angle when using the curvature size function type.

. If applicable, deselect Ignore Self when using the proximity size function type. By default, Ignore Self

is enabled, such that the proximity between two facets belonging in a single face zone will be ignored,

avoiding unnecessary over-refinement.

. Choose an option in the Scope Proximity To field, where the size controls can be scoped to edges, faces,

or to both faces and edges. Note that if you select faces-and-edges, you can only select objects.

available zones in the list before selecting a zone. Note that this option is not applicable when Scope

Proximity To is set to faces-and-edges.

. Select the Show Size Box field to visualize the size control's minimum and maximum sizes in the graphics

window (in the form of red cubes).

Specify a value for the Wrap Min Size field.

Specify a value for the Wrap Max Size field.

Select the Show Wrap Size Box field to visualize the wrap's minimum and maximum sizes in the

graphics window (in the form of red cubes).

. Once your selections are made, click Setup Size Controls and proceed onto the next task.

The Generate the Surface Mesh task will close all the leakages to objects and void regions and then

generate only the surface mesh.

If required, specify the Surface Mesh Target Skewness, or keep the default setting. This value is the

target maximum surface mesh quality, and is recommended to be between . and ..

For Advanced Options, you can:

Indicate whether or not you want to save intermediate files. Select Yes if you want to save files after

each major operation such as computing size field, wrapping, surface remesh, etc.This is useful when

meshing large models so that you can load those files of interest during the meshing process.

Indicate whether or not you want to separate the surface mesh. Select Yes if you want to have the final

surface mesh to be viewed as separated zones.

Indicate whether or not you want to separate contact pairs between fluids and solids in the

Indicate whether or not you want to perform solid meshing using parallel sessions. Select Yes

and indicate the Maximum Number of Sessions. The number of parallel sessions that are used

will depend upon the number of solid objects that need to be meshed. For example, if you in-

dicate four parallel sessions, and you want to mesh three solid objects, then three parallel ses-

sions will be used to perform the solid meshing. If, however, you have six solid objects that

need to be meshed, then they will be equally divided between the four parallel sessions.

Once your selections are made, click Generate the Surface Mesh and proceed onto the next task.

If you need to make adjustments to any of your settings in this task, click Revert and Edit, make your

For most fluid regions, the boundary layer flow along the walls of the geometry is best captured using

specialized boundary layer elements within the volume mesh (also called prisms or inflation layers).

Prism elements are generated on the walls of the geometry that face the fluid region (typically referred

to as “wetted” walls). You can use the Setup Boundary Layers task to assign different regions to have

their own boundary layer controls. When a boundary layer is assigned to a region, all face zones asso-

ciated with that region will be assigned those settings. Any zone-specific settings (except the number

of layers) defined in the Prisms dialog are respected. For more information about prisms, see Generating

Prisms (p. ) and Growth Options for Zone-Specific Prisms (p. ).

For the Would you want to add boundary layers to fluid regions? field, select yes if your model

requires you to locate and address any boundary layers using the following steps. Otherwise, if your

model does not require you to have boundary layers, keep the default of no, click Update and proceed

. Specify a Name for the boundary layer control, or use the default name (prism-).

. Choose an Offset Method Type.The offset method that you choose determines how the mesh cells

closest to the boundary are generated. See Offset Distances (p. ) for more information. Choices include:

aspect-ratio: allows you to control the aspect ratio of the boundary layer cells (or prism cells) that are

extruded from the base boundary zone.

Specify the Aspect Ratio that you want to use for the boundary layer. The aspect ratio is defined

as the ratio of the prism base length to the prism layer height.

last-ratio: allows you to specify the cell size ratio between the last layer and base cell of the boundary

layer cells (or prism cells) that are extruded from the base boundary zone.

– You can specify a value for the First Height, which corresponds to the height of the first layer of cells

in the boundary layer.

– You can specify a value for the Last Ratio Percentage.

uniform: allows you to generate every new node (child) to be initially the same distance away from its

parent node (that is, the corresponding node on the previous layer, from which the direction vector is

pointing).

. Specify a value for the Growth Rate.This value determines the relative thickness of adjacent inflation

layers. As you move away from the face to which the inflation control is applied, each successive layer is

approximately one growth rate factor thicker than the previous one.

. Use the Region list to select the region that requires a boundary layer control.

. Once your selections are made, click Setup Boundary Layers and proceed onto the next task.

The Generate the Volume Mesh task will perform various operations and generate the volume mesh.

If required, specify the Volume Mesh Target Skewness, or keep the default setting. This value is the

target maximum volume mesh quality, and is recommended to be around ..

If you would like to review and change the volume meshing technique for your region(s), you can select

the Edit Volume Fill Settings option. This displays a tabular overview of the simulation's volume re-

gion(s) and their mesh settings (formerly set in the Update Region Settings task), that you can change

accordingly before finally generating the volume mesh.

Once your selection is made, click Generate the Volume Mesh and proceed onto the next task.

From this task, if you need to address any surface contact issues, you can add a Separating Contacts

task to your workflow (see Separating Contacts (p. )).

Once you have completed the volume mesh, you can add the Separate Contacts task to address any

issues with contact surfaces and separate any contacts between fluid cell zones (fluid regions).

. Use the Separate Contacts field to enable or disable the ability to separate any existing contacts between

surfaces.

. Once your selections are made, click Separate Contacts to update the task.

Upon completion, the task will generate a Scheme file called out_solver_f2f_set_nci.scm.

This Scheme file can be loaded into the Fluent solver after mesh scaling (File > Read > Scheme),

which will automatically set the mesh interfaces.

Chapter : CAD Assemblies

The CAD Assemblies mode offers additional tools for imported CAD data in Fluent Meshing. The CAD

Assemblies tree represents the CAD tree as it is presented in the CAD package in which it was created.

All sub-assembly levels from the CAD are maintained on import in Fluent Meshing.

Advantages of using the CAD Assemblies tree include the following:

The CAD assemblies tree enables faster visualization which saves time in part management for large, complex

models comprising multiple assemblies.

It enables re-importing or updating of selected parts or bodies using different faceting qualities and topology

representations from a neutral database file.

Geometry and mesh objects can be easily created for only those assemblies, parts, or bodies that are needed

for the analysis. Other assemblies, parts, or bodies can be simply suppressed.

The geometry and mesh objects are linked to the corresponding CAD objects (which are then locked), enabling

quick design changes and updates.

Labels can be assigned to entities, and these are preserved throughout the object-based meshing workflow

in Fluent Meshing.

The use of CAD assemblies for CAD import in Fluent Meshing is described in the following sections.

.. CAD Assemblies Tree

..Visualizing CAD Entities

.. Updating CAD Entities

.. Manipulating CAD Entities

.. CAD Association

The CAD Assemblies tree is created when the Create CAD Assemblies option is selected for CAD import.

It represents the CAD tree as it is presented in the CAD package in which it was created. All sub-assembly

levels from the CAD are maintained on import in Fluent Meshing.

To create the CAD Assemblies tree on import, enable Create CAD Assemblies in the Object Creation

group box in the CAD Options dialog box. The CAD object and zone granularity can be specified in

the Object Creation group box. You can choose to create one CAD object per part, body, CAD file or

selection imported. Similarly, you can choose to create one CAD zone per body, face, or object imported.

Tip

Importing CAD objects by body gives an ideal CAD assemblies tree, with the original sub-

assemblies preserved.

The CAD assemblies tree includes individual CAD assemblies or sub-assemblies imported in Fluent

Meshing. The entity at the highest level is also referred to as the root node.

The CAD entities in the tree are categorized as components and bodies. Components represent an

assembly, sub-assembly, or part in the original CAD package, while bodies are the basic entities in the

CAD assemblies tree which include CAD zones. You can also set up labels for the CAD zones, if required.

Named Selections are also imported as labels. These labels are preserved throughout the object-based

meshing workflow in Fluent Meshing.

In addition to the context-sensitive menus, you can manage the CAD entities using hotkeys or onscreen

tool buttons. Tools exist for visualizing the CAD entities, for operations such as updating and modifying

the CAD entities, creating and/or modifying geometry or mesh objects, and tree selection options. See

Appendix C: Shortcut Keys (p. ) for more information.

Note

At the global CAD Assemblies level, you can use the menu options to draw or delete all the assemblies

imported, and obtain the locations of the referenced FMDB files. The Tree sub-menu contains options

for navigation and selections in the tree.

... FMDB File

... CAD Entity Path

... CAD Assemblies Tree Options

The FMDB file (*.fmdb) is a CAD neutral file that is created when the CAD Assemblies are created

during CAD import. This file enables quick re-import of the CAD data with changes to the faceting

qualities and/or topology representations.

When importing a single file, the FMDB file is created in the folder containing the CAD file and has the

same name as the file imported.

When importing multiple files, the FMDB file is created in the folder containing the CAD files and is named

multiple.fmdb by default.You can specify an appropriate name in the FMDB Location dialog box

when prompted.

The menu at the global CAD Assemblies level enables you to obtain a list of the referenced FMDB files.

Select Referenced FMDB in the menu to open the Referenced FMDB files dialog box containing the

list of FMDB files.

All CAD entities and labels in the CAD Assemblies tree are referred to by their path. The path is used

in commands in the cad-assemblies menu (see cad-assemblies/ for details).

To see the path, right-click the CAD entity in the tree and select Tree → Show Path.

Examples of the CAD entity path:

|assembly.agdb|component_1

CAD Assemblies

|assembly.agdb|component_1|body_1

|assembly.agdb|body_1|label

The Tree menu contains options that control the appearance of the CAD Assemblies tree. These options

can be used to select or deselect the CAD objects and zones in the tree, expand or collapse the tree

branches, and also delete suppressed or locked CAD objects.

At the global CAD Assemblies level:

The Selection Helper enables you to select or deselect CAD objects or labels in the tree based on the

specified Name Pattern.You can choose cad-objects, leaf-cad-objects, non-leaf-cad-objects, or label

in the Filter list.

The Select Next Level option selects the CAD assemblies or objects at the next lower level.

The Collapse All option collapses the tree to the level selected.

The Delete Locked/Suppressed option deletes all locked or suppressed CAD assemblies or objects.

The Restore Deleted option restores previously deleted CAD assemblies or objects.

At the component level:

The Selection Helper enables you to select CAD objects or labels in the tree based on the specified Name

Pattern.You can choose leaf-cad-objects, non-leaf-cad-objects, or label in the Filter list.

The Expand All option expands the tree to show all subsequent levels (CAD objects and labels, if applicable).

Similarly, the Collapse All option collapses the tree to the level selected.

The Show Path option prints the CAD entity path in the console.

The Suppress Other option suppresses all other CAD entities at the same level.

The Select Associated Objects selects geometry/mesh objects associated with the selected component.

At the body level:

The Select Associated Objects selects geometry/mesh objects associated with the selected body.

At the label level:

The Select All Parent option selects all the parent CAD entities in the tree.

CAD Assemblies Tree

CAD entities can be displayed using the options available for the CAD Assemblies tree:

The global menu for the CAD Assemblies contains an option to draw all the CAD assemblies imported.

The menu for individual components and bodies contains an option to draw the selected entity.You can

also use the additional options in the Draw Options menu to add, remove, or highlight the selected entity

in the display.You can also draw the unlabeled zones for the entity selected.

The menu for labels contains an option to draw the selected label.You can also use the additional options

in the Draw Options menu to draw all labels and add, remove, or highlight the selected label in the display.

You can also draw the overlapping zones for the label selected.

The CAD entities are displayed using a different color palette to that used for the geometry/mesh objects.

The zone and object selection filters also apply to the CAD zones and objects.

Other visualization tools and shortcuts are also applicable to the CAD entities. You can use the shortcut

keys or onscreen tools to select visible entities, deselect all or the last selected entity, hide/show entities.

You can also use the Isolate tools to isolate selected entities in the display or limit the display to entities

based on area/curvature of the selected entities.

The Update option enables reimporting the CAD entities using new parameters. Select the CAD objects

in the tree and select Update. Alternatively, select the CAD objects in the graphics display and click

to open the Update dialog box.

Tip

Be sure to clear the tree (using Ctrl+Y) before selecting items to update.

You can change the CAD zone granularity, if required.

Select the Tessellation option and specify the tessellation controls:

– If you select the CAD Faceting option, you need to specify the Tolerance for refinement and the Max

Size in the CAD Faceting Controls group box.The default value for Tolerance is , which implies no

tessellation (faceting) refinement during import.The Max Size enables you to specify a maximum facet

size for the imported model to avoid very large facets during the file import.

(Min Size, Max Size), and the curvature normal angle to be used for refining the surface mesh based on

the underlying curve and surface curvature.You can optionally use the edge proximity size function for

creating the surface mesh, based on the number of cells per gap specified.You can also choose to save

a size-field file based on these defined parameters (i.e., Min Size, Max Size, Curvature Normal Angle, Cells

Per Gap). Note that for proximity size functions, the number of cells per gap can be a real value, with a

minimum of . (see Proximity (p. ) for more information).

Use Size Field File.

You can choose to import edge zones from the CAD entities. Specify an appropriate value for Angle.

CAD management operations are available from the tree menus as well as through the graphics icons

and hot-keys.

... Creating and Modifying Geometry/Mesh Objects

... Managing Labels

... Setting CAD Entity States

... Modifying CAD Entities

The Object menu contains options for creating geometry/mesh objects from the CAD entities and

modifying existing objects. Select the CAD entities in the tree and then choose the appropriate menu

option. Alternatively, select the CAD objects in the graphics display and select the option from the

CAD Tools.

Use the Create (

) option to create a new geometry/mesh object.The Create Object dialog box contains

options for creating a geometry or mesh object based on the tree selections. Specify the Object Name,

Object Type (geom or mesh), and the Cell Zone Type (solid, fluid, or dead). In case of multiple selections,

you can choose to create One Object per CAD Object Selection.You can also choose to retain the CAD

zone granularity by enabling Keep CAD Zones Granularity.

Note

The CAD association will be transferred to the objects when you choose to retain the

CAD zone granularity for object creation.

Use the Add to (

) option to add the selected CAD entities to an existing object.The Add to Object

dialog box contains a list of the current objects. Select the object to be modified and click Add.

When CAD entities are added to an object, the zones are merged to create a single zone. If the CAD

entities have labels defined:

– Adding the entities to an object with no labels defined will result in the labeled zones retained as separate

zones.

– Adding the entities to an object with the same labels defined will result in the labels being merged, but

retain the zones retained as separate zones.

Use the Replace option (

) to replace an existing object with the selected CAD entities.The Replace

Object dialog box contains a list of the current objects. Select the object to be replaced and click Replace.

Manipulating CAD Entities

You can set up labels for the CAD zones, if required. Named Selections are also imported as labels.

These labels are preserved throughout the object-based meshing workflow in Fluent Meshing.

You can manage labels for CAD entities using the Manage Labels dialog box. Select the CAD zones

in the display using the zone selection filter (

) and then click Manage Labels (

).

Use the Create/Add label option to create a new label for the CAD zones selected and click Add. If Remove

).

CAD Zones from Graphics is enabled (default), the selected CAD zones will be removed from the display

after the label is created.

Use the Create/Add label option to add an existing label to the CAD zones selected. Select the labels from

the list and click Add. If Remove CAD Zones from Graphics is enabled (default), the selected CAD zones

will be removed from the display after the zones are added to the label.

Use the Remove label option to remove an existing label from the CAD zones selected. Select the labels

from the list and click Remove.

The Modify menu for labels contains options for deleting and renaming labels.

Use the Delete option to delete the selected labels.

Use the Rename option to rename the labels.Specify the name in the Rename Labels dialog box and click

OK. In case of multiple selections, the specified name will be used, with a suitable index as suffix. For example,

specifying a new label name wall will result in labels wall., wall., etc.

The State menu for the CAD entities (component or body) contains options for setting the CAD entity

state.

Locked

CAD entities are locked when corresponding geometry or mesh objects are created. Locked entities

cannot be modified or used for creating objects.This prevents the use of the same CAD entity in multiple

objects.

To unlock an entity, use the State → Unlock option.

Suppressed

CAD entities can be suppressed if they are not required for the analysis.You can transfer only necessary

objects.

entities to geometry or mesh objects for meshing using the object-based workflow and suppress the re-

maining entities.

To suppress an entity, use the State → Suppress option. Alternatively, select the CAD objects and

click

.

To unsuppress an entity, use the State → Unsuppress option.

The options in the Modify menu at the CAD entity (component or body) level enable modifying the

CAD entities. Select the CAD entities in the tree and then choose the appropriate menu option. Altern-

atively, select the CAD objects in the graphics display and select the option from the CAD Tools.

Use the Extract Edge Zones option (

) to extract the feature edge zone for the selected entities. Specify

the Angle in the Extract Edge Zones dialog box and click Create.

Use the Rename  (

) option to rename the selected entities. Specify the name in the Rename CAD

Assemblies dialog box (or the Rename Entities dialog box) and click OK. For multiple entities, the specified

name will be used, with a suitable index as suffix. For example, specifying a new name wall will result in

entities wall., wall., etc.

Use the Add Prefix  option to add a prefix to the selected entities. Specify the prefix in the Prefix name

dialog box and click OK.

The CAD Association menu for geometry/mesh objects contains options for modifying the selected

objects based on the associated CAD entities. You can also attach or detach the CAD entities from the

objects.

objects.

Use the Update from CAD option to update the geometry/mesh objects based on changes to the associated

CAD objects.

Use the Unlock CAD option to unlock the CAD objects associated with the selected geometry/mesh objects.

Use the Select CAD option to select the CAD objects associated with the selected geometry/mesh objects.

Use the Detach CAD option to detach the CAD objects associated with the selected geometry/mesh objects.

All association will be removed and the geometry/mesh objects will be independent of changes to the CAD

entities.

Use the Attach CAD option to attach CAD objects to the selected geometry/mesh objects. Select CAD objects

to be associated with the geometry/mesh objects in the tree and click Confirm in the Attach CAD assemblies

dialog box.The selected geometry/mesh objects will be associated with the CAD objects which will then

be locked.

Use the Restore CAD option to restore the geometry/mesh object from the associated CAD objects.

CAD Association

Chapter : Size Functions and Scoped Sizing

Size Functions and Scoped Sizing provide control over how the mesh size is distributed on a surface

or within the volume. They provide accurate sizing information for the mesh distribution and precise

refinement control.

Scoped sizing differs from size functions in how the sizing can be associated with objects or zones, re-

spectively. Scoped sizing may be applied to model features such as faces, edges, face zone labels or

unreferenced face or edge zones. You can optionally select the type of object (geom, mesh) while ap-

plying scoped sizing. Scoped sizing can be defined on individual zone or object entities by selecting

from a list or using wildcards (*). For convenience, your scoped sizing definitions can also be saved to

a file (*.szcontrol) which can be read in and reused for similar models having the same naming

conventions.

The size field is computed based on the size functions and/or scoped sizing defined. You can remesh

surfaces and edges based on the size field. The CutCell mesher also uses the size field to refine the

initial Cartesian mesh.

Important

Size functions can be computed only for triangulated zones. For zones comprising non-trian-

gular elements, you can triangulate the zones manually before computing the size functions.

Alternatively, you can use the command triangulate-quad-faces? before computing

the size functions. This command identifies the zones comprising non-triangular elements

and uses a triangulated copy of these zones for computing the size functions.

When the size functions or scoped sizing is used, the mesh distribution is influenced by

The minimum and maximum size values

The growth rate

The size source which can be any one of the following:

– Edge and face curvature, based on the normal angle variation between adjacent edges or faces.

– Edge and face proximity, based on the number of element layers created in a gap between edges or faces.

– The body of influence defined.

– Constant user-defined sizes through hard and soft behaviors.The curvature, proximity, body of influence,

and soft size functions have soft behavior.The meshed and hard size functions have hard behavior.

This chapter contains the following sections:

..Types of Size Functions or Scoped Sizing Controls

.. Defining Size Functions

.. Defining Scoped Sizing Controls

.. Computing the Size Field

.. Using the Size Field

The following size functions or scoped sizing controls are available:

... Curvature

... Proximity

... Meshed

... Hard

... Soft

... Body of Influence

The curvature size function/scoped control computes edge and face sizes using their size and normal

angle parameters, which are either automatically computed or defined.

The curvature sizing is defined by the following parameters:

Min, Max size

Growth rate

Normal angle

The curvature size function/scoped control uses the normal angle parameter as the maximum allowable

angle that one element edge may span. For example a value of  implies that a division will be made

when the angle change along the curve is  degrees; hence, a  degree arc will be divided into ap-

proximately  segments.

Note

As the curvature values are computed approximately using edges and face facets, there

may be some numerical errors, especially when face facets are excessively stretched.

Figure . : Use of Curvature Sizing (p. ) shows an example where the surface has been remeshed

based on a curvature size function. The change in normal angle and growth rate controls the size

distribution.

Size Functions and Scoped Sizing

Figure . : Use of Curvature Sizing

The proximity size function/scoped control computes edge and face sizes in ‘gaps’ using the specified

minimum number of element layers. For the purposes of specifying proximity sizing, a ‘gap’ is defined

in one of two ways:

The area between two opposing boundary edges of a face

The internal volumetric region between two faces

The proximity sizing is defined by the following parameters:

Cells per gap

Figure . : Use of Proximity Sizing (p. ) shows an example where the surface has been remeshed

based on a proximity size function. The change in the cells per gap and growth rate parameters control

the size distribution.

Types of Size Functions or Scoped Sizing Controls

Figure . : Use of Proximity Sizing

Note

For proximity size functions, the number of cells per gap can be a real value, with a minimum

of .. This has the effect of increasing the size of face elements located farther away from

edges, and stretching face elements with larger sizes along side faces, or gaps, thereby re-

ducing the overall face count, and ultimately the cell count.

Additional options for defining the face proximity sizing are as follows:

The Face Boundary option enables you to compute the shell proximity (edge-edge proximity within each

face).The proximity between feature edges on the face zones selected is computed.This option is particularly

useful for resolving trailing edges and thin plates without using the hard size function.

The example in Figure . : Use of the Face Boundary Option for Face Proximity (p. ) shows the

use of this option for a blade configuration. Though the normals on the blade surface point outward,

the cells across the trailing edges will be refined based on the proximity size function defined for

the trailing surfaces when the Face Boundary option is enabled.

Figure . : Use of the Face Boundary Option for Face Proximity

Note

The Face Boundary option works on the internally extracted boundary edge zones of

the face zones. Edge zones extracted in the meshing mode/CAD imported edges will not

be considered for the proximity calculation.

The Face - Face option enables you to compute the proximity between two faces in the face zones selected.

When the Face - Face option is enabled, additional options for ignoring self proximity (Ignore Self) and

ignoring the face normal orientation (Ignore Orientation) are also available.

The Ignore Self option can be used with the Face - Face option in cases where self proximity

(proximity between faces in the same face zone) is to be ignored. This option is disabled by default.

The Ignore Orientation option can be used to ignore the face normal orientation during the prox-

imity calculation. This option is enabled by default. In general, the proximity depends on the direction

of face normals. An example is shown in Figure . : Use of the Ignore Orientation Option for Face

Proximity (p. ). The normals on the grooved box point inward. With only the Face - Face option,

the proximity size function does not refine the surface along the entire groove length. When the

Ignore Orientation option is enabled along with the Face - Face option, the surface will be refined

along the groove length.

Figure . : Use of the Ignore Orientation Option for Face Proximity

Note

You must select at least one of the Face Boundary and Face - Face options; otherwise, an

error will be reported.

Note

The edge proximity size function depends only on the distance between the edges, irrespective of

their association with a face zone or the orientation of the face zones associated with the edge zones.

Important

When using a proximity sizing in certain geometries (with angle >  degrees or comprising

extended region of non-intersecting faces), the proximal face zones may not be detected

and may result in a warning message. In such cases, split the proximity sizing into multiple

proximity scoped sizing controls.

Tip

When using a proximity size function with geometries having a very large number of small

feature edges, you can speed up the calculation and reduce memory requirements by en-

abling Quick Edge Proximity. Go to Display → Controls, select Size Functions from the

Categories drop down list, and check Quick Edge Proximity. Accuracy will be reduced

when Quick Edge Proximity is enabled.

... Meshed

The meshed size function/scoped control enables you to set the size based on existing sizes. This

provides gradation between the minimum and maximum size based on the specified growth rate.

The default behavior for the meshed size function/scoped control is soft, allowing other hard sizes or

locally smaller sizes to override it. You can enable Hard Meshed Size Functions by going to the Display

> Controls menu, and selecting Size Functions in the drop down list.

Note

In Release . and earlier, the behavior for the meshed size function/scoped control was

Note

hard. This behavior is saved with the mesh file. Therefore, when reading a mesh saved using

such a release, the Hard Meshed Size Functions control may be enabled.

The meshed sizing is defined by the growth rate.

In Figure . : Use of Meshed Sizing (p. ), the face zone is remeshed based on the premeshed face

zone indicated.

Figure . : Use of Meshed Sizing

... Hard

The hard size function/scoped control enables you to maintain a uniform size based on the size specified,

while the growth rate from the defined size influences the size on adjacent zones. The hard sizing will

override any other size function specified.

The hard sizing is defined by the following parameters:

Min Size

Important

It is recommended to not have two hard sizes next to each other as the mesh size transition

between the two will not be smooth.

If two hard sizes are applied at the same location, the latter will be honored.The smaller size

rule does not apply in this case.

... Soft

The soft size function/scoped control enables you to set the maximum size on the selected zone, while

the specified growth rate from the defined size influences the size on adjacent zones. When the soft

sizing is selected for edges and/or faces, the size will be affected by other size functions/scoped controls.

The minimum size on the zone will be determined based on the influence of other size functions/scoped

controls, else a uniform size will be maintained. In other words, a soft sizing is ignored in a region

where other sizing controls specify smaller sizes.

The soft sizing is defined by the following parameters:

Max size

In the example in Figure . : Use of Soft Sizing (p. ), the minimum size is determined by the hard

sizing applied on the smaller face zones indicated, and maximum size is limited by the soft sizing ap-

plied.

Figure . : Use of Soft Sizing

The body of influence size function/scoped control enables you to specify a body of influence (that

is, a region for sizing control). The maximum mesh size will be equal to the specified size within the

body of influence. The minimum size will be determined based on the influence of other size func-

tions/scoped controls. An example is shown in Figure . : Use of Body of Influence Sizing (p. ).

Note

The set of face zones selected to define the body of influence should constitute a geomet-

rically closed region. If an open region is used as a body of influence, the sizing will be

processed as a soft sizing.

The body of influence sizing is defined by the following parameters:

Max Size

In Figure . : Use of Body of Influence Sizing (p. ), the mesh is generated based on the body of in-

fluence sizing defined. The finer mesh size is obtained due to other size functions (for example,

curvature, proximity) defined in addition to the body of influence size functions.

Figure . : Use of Body of Influence Sizing

Important

In case of multiple non-intersecting closed bodies, a single BOI size function/scoped sizing

control can be set up.The sizing can be scoped to the set of face zones comprising the respective

bodies.

bodies.

In case of multiple intersecting closed bodies for scoping the same BOI sizing, you need to create

separate BOI size functions/scoped sizing controls for each geometric body.

Note

When using BOIs with periodic boundaries, if the BOI extends outside the domain, it may

cause unnecessary refinement.

Size functions can be defined using the Size Functions dialog box. Right-click on Model in the tree

and select Functions... from the Sizing menu. The generic procedure to define size functions is as follows:

Defining Size Functions

.

Ensure that the global controls are set as required.The relevant size function parameter values (minimum

and maximum size, growth rate) will be updated based on the global controls specified.

.

Enable Face Zones (or Edge Zones) as appropriate.

.

Select the boundary zones (or the edge zones) for which the size function is to be defined in the Boundary

Zones (or Edge Zones) selection list.

Note

All boundary face zones and edge zones included in the global domain are available

for defining size functions, even if a local domain has been activated.

.

Select the appropriate size function type in the Size Function Type drop-down list in the Define Size

Function group box.

.

Enter an appropriate size function name in the Name field or leave the field blank if you want to have

the name generated automatically. In this case, the Name will be assigned according to the zone type

(face or edge) and the size function type. (For example, face-curvature-sf- indicates that the curvature

size function is defined for face zones.The size function ID is .)

.

.

Specify the size function parameters applicable for the selected size function as appropriate and click

Create.

The defined size function will be available in the Size Functions list.

... Creating Default Size Functions

You can create default size functions based on face and edge curvature and proximity using the Create

Defaults option in the Size Functions dialog box. Alternatively, you can use the command /size-

functions/create-defaults to create the default size functions.

The following size functions will be defined:

Curvature size function on all edge zones, with the global minimum and maximum sizes and growth rate,

and a normal angle of .

Curvature size function on all face zones, with the global minimum and maximum sizes and growth rate,

Proximity size function on all edge zones, with the global minimum and maximum sizes and growth rate,

and the cells per gap set to .

Proximity size function on all face zones, with the global minimum and maximum sizes and growth rate,

When the Create Defaults option is used after the default size functions have been created, the pre-

vious definitions will be updated based on any changes to the global minimum and maximum sizes

and growth rate.

Scoped sizing controls can be defined using the Scoped Sizing dialog box. Right-click on Model in the

tree and select Scoped... from the Sizing menu. The generic procedure for defining scoped sizing

controls is as follows:

.

.

Set the global scoped sizing controls as required.The relevant local control parameter values (minimum

and maximum size, growth rate) will be updated based on the global values specified.

.

Select the appropriate scoped control type in the Type drop-down list in the Local Scoped Sizing group

box.

.

Enter an appropriate name in the Name field.

.

Specify the local sizing parameters applicable for the selected scoped control type as appropriate.

.

Select the scope for the scoped control defined from the Scope To drop-down list. Additionally, select

the Object Type (Geom and/or Mesh) and specify a suitable pattern in the Selections field.

You can also click

to open the Scope dialog box and select the objects, face zone labels, face

zones, or edge zones for defining the size control scope.

.

Click Create New.

The defined size control will be available in the Controls list.

You can validate the defined scoped sizing controls using the command /scoped-sizing/validate.

An error will be reported if the scoped sizing controls do not exist or the scope for one (or more) controls

is invalid.

... Size Control Files

The size controls file (*.szcontrol) contains the scoped sizing control definitions. The control name

and type, and the scope of the control will be included in the size control file along with global size

parameters.

To read a size controls file, click Read... in the Scoped Sizing dialog box to invoke the Select File

dialog box and specify the name of the file to be read. Alternatively, you can use the /scoped-

sizing/read command and specify the name of the file to be read.

To write a size controls file, click Write... in the Scoped Sizing dialog box to invoke the Select File

dialog box and specify the name of the file to be written. Alternatively, you can use the /scoped-

sizing/write command and specify the name of the file to be written.

The size field can be computed based on the defined size functions and scoped sizing controls by

clicking Compute in the Size Functions dialog box or the Scoped Sizing dialog box. Alternatively, use

Computing the Size Field

the command /size-functions/compute or /scoped-sizing/compute to compute the size

field.

Important

If the size field has been computed in the current session, sizes will be based on the computed

size field. You cannot define additional size functions or scoped sizing controls, or modify

the current sizes without deleting the size field.

... Size Field Files

Size field files contain the size function definitions based on the parameters specified.

Select the File/Read/Size Field... menu to read a size field file. This will invoke the Select File dialog

box, where you can specify the name of the size field file to be read. Alternatively, you can use the

/file/read-size-field command and specify the name of the file to be read.

Important

If a size field file has been read in the current session, sizes will be based on the size field

read. You cannot define additional size functions or scoped sizing controls, or modify the

current sizes without deleting the size field.

Select the File/Write/Size Field... menu to save a size field file based on the parameters set. This will

invoke the Select File dialog box, where you can specify the name of the size field file to be written.

Alternatively, you can use the /file/write-size-field command and specify the name of the

file to be written.

... Using Size Field Filters

Additional size field filtering options are available after the size field is computed/read. These options

are available in the Size Field Filters dialog box.

Click Filters... in the Size Functions or Scoped Sizing dialog box to open the Size Field Filters dialog

box.

You can specify a scale factor to filter the size output from the size field, without deleting and recomputing

the size field.The scaling filter can be applied as follows:

.

Specify an appropriate value for Factor, Min and Max (for Scale).

.

Click Apply.

Alternatively, you can use the command /size-functions/set-scaling-filter, and specify

the scale factor, minimum and maximum size values.

You can apply periodicity to the size field, without deleting and recomputing the size field as follows:

.

Click Set... to open the Periodicity dialog box.

.

Select the type of periodicity (Rotational or Translational).

.

For translational periodicity, specify the shift vector components You can also click Define and select

nodes to set up the shift vector for translational periodicity.

.

For rotational periodicity, enter an appropriate value for Angle.

.

For rotational periodicity, specify the pivot point and axis of rotational periodicity.

You can also select – nodes and click Define to set up the pivot point and axis of rotation

.

for rotational periodicity as follows:

– If only  node is selected, the pivot point is at the node location and the axis of rotation is the

global z-axis.

– For  nodes, the pivot point is at the midpoint of the nodes selected and the axis of rotation is the

– For  nodes, the pivot point is at the first node selected.The axis of rotation is the local z-axis normal

to the plane defined by the three points, the positive direction is determined by the right-hand rule.

– For ,  or  nodes, the first  points define a circle.The pivot point is at the center of the circle.The

axis of rotation is the local z-axis normal to the circular plane, the positive direction is determined

by the right-hand rule.

.

Click Apply to enable Periodicity in the Size Field Filters dialog box.

Note

– If periodicity is set up prior to computing the size-field, the Periodicity filter will be en-

abled when the size-field is computed.

Alternatively, you can set up the periodic boundary using the Make Periodic Boundaries dialog

box. See Creating Periodic Boundaries (p. ) for details.

Boundary → Create → Periodic...

You can also use the command /size-functions/enable-periodicity-filter and specify

the angle, pivot, and axis of rotation. If periodicity has been previously defined, the existing settings

will be applied.

...Visualizing Sizes

Before computing the size field, you can check if the global minimum and maximum sizes are suitable

locally. After computing the size field, you can set the selection filter to size and use the probe to

determine local size or make a contour plot of the sizing on any surface

You can display the contours of size using the options in the Size Functions dialog box as follows:

.

Select the face zones in the Boundary Zones selection list in the Size Functions dialog box.

.

Specify appropriate values for Min and Max in the Contours group box.

.

Click Draw (in the Contours group box).

Alternatively, after selecting the face zones, use the hot key Ctrl+T (Miscellaneous Tools), then Ctrl+C

to draw size contours.

Figure . : Contours of Size (p. ) shows the display of contours of size on the selected face zones

after the size field has been computed or read

Figure . : Contours of Size

A visual indication of mesh size is also available using the mouse probe.

Size selection filter

If the selection filter is set to size (hot key Ctrl+Y), right-click at the required locations to see the size

boxes indicating the mesh size. See Figure . : Display of Mesh Size Based on Size Field (p. ).

Figure . : Display of Mesh Size Based on Size Field

Preview sizes

Alternatively, after selecting the face zones, use the hot key Ctrl+T (Miscellaneous Tools), then Ctrl+P to

preview sizes on the selected zones.You can set the minimum and maximum size values in the Preview

Sizes dialog box.

The size field can be used to remesh surfaces and edges. The CutCell mesher also uses the size field to

refine the initial Cartesian mesh.

Remeshing Surfaces

The generic procedure for remeshing surfaces is as follows:

.

.

Select the surface(s) to be remeshed.You can use the graphics select tools or select from a list in a dialog

box.

.

Use the hotkey Ctrl+Shift+R or click the Remesh button to open the Zone Remesh dialog box.

.

Choose the appropriate Sizing from the drop down list and set other parameters as necessary.

.

Click Remesh.

For more control of surface remeshing parameters, use the Surface Retriangulation dialog box as follows:

Boundary → Mesh → Remesh

.

Select the surfaces to be remeshed in the Face Zones list.

.

Enable Size Function in the Face Remesh Options group box and click the Specify button to open the

Size Functions dialog box and check that the size functions are appropriate. See Defining Size Func-

tions (p. ).

Alternatively, ensure that the size field has been computed or read in.

.

Set the other options for face remeshing as appropriate.

.

Important

Edge zones associated with face zones are not remeshed implicitly. If you have feature

edge zones associated with the surface being remeshed, you need to remesh them before

remeshing the face zones.

Remeshing Edges

The generic procedure for remeshing edges is similar to the above procedure for surfaces. Use the

hotkey Ctrl+Shift+Z, or click the Edge Zone restriction button, to constrain the selection to edge zones

only.

For more control of edge remeshing parameters, use the Feature Modify dialog box as follows:

Boundary → Mesh → Feature

.

Ensure that the edge zones are extracted as required.

.

Select the edges to be remeshed in the Edge Zones list in the Feature Modify dialog box.

.

.

.

.

Select Remesh in the Options list and select Size Function in the Method drop-down list.

.

Make sure the size functions are defined as appropriate in the Size Functions dialog box (see Defining

Size Functions (p. )). Alternatively, ensure that the size field has been computed or read in.

Using the Size Field

.

Refining the CutCell Mesh

The CutCell mesher uses the size functions/size field to refine the initial Cartesian mesh as described

in The CutCell Meshing Process (p. ).

Chapter : Objects and Material Points

This chapter describes the use of objects and material points for identifying the mesh region.

.. Objects

.. Material Points

.. Objects

An object—generally a set of face zones and edge zones—is used to identify the domain to be meshed.

By including edge zones in the object definition, you are able to capture the object features even when

wrapping.

Objects are generally closed solid volumes, closed fluid (wetted) volumes, capping surfaces, or individual

face zones that can be used for meshing. For example, using capping surfaces in conjunction with a

material point and a closed solid volume enables you to extract the flow volume using wrapping.

Objects (defined or imported) are independent of each other; that is, objects do not share face and/or

edge zones. In cases where objects are defined using a common face/edge zone, the common face/edge

zones are duplicated to make the objects independent.

Object Based Meshing

Objects can be used for mesh generation as described:

Surface Meshing

Object wrapping or join and intersect operations are used to create a conformal, connected surface mesh.

This is the first of a two-step process for creating a tetrahedral, hexcore, polyhedral, or hybrid mesh in

meshing objects.This process is described in Object-Based Surface Meshing (p. ).

Volume Meshing

The Volumetric Regions are calculated from the conformal, connected surface mesh, and then filled with

tetrahedral, hexcore, or polyhedral mesh, with or without inflation layers.This is the second of a two-step

process for meshing objects and is described in Object-Based Volume Meshing (p. )

Auto Mesh

An object-based workflow to generate a volume mesh.You can select the desired mesh object in the

Model tree and select Auto Mesh... from the menu available. Alternatively, use the Mesh → AutoMesh...

menu to open the Auto Mesh dialog box, then select the mesh object in the Object drop-down list.

See Using the Auto Mesh Dialog Box (p. ) or Meshing All Regions Collectively Using Auto

Mesh (p. ) for details on using the Auto Mesh dialog box.

Note

The No Fill option is not available when a mesh object is selected for volume

meshing.

Auto Fill Volume

A selective workflow to generate a volume mesh on selected volumetric regions.You can select the

desired Volumetric Regions in the Model tree and select Auto Fill Volume from the menu available.

See Meshing Regions Selectively Using Auto Fill Volume (p. ).

CutCell Meshing

A general purpose, hex-dominant meshing technique using a direct surface and volume approach. Objects

can be used to determine the inclusion of Cartesian grid entities for CutCell meshing.The Cartesian grid

will be refined and snapped to any face zone included in the objects selected for CutCell meshing. See

Generating the CutCell Mesh (p. ).

Objects descriptions include attributes (type, cell zone type and priority) and entities (face zone labels,

volumetric regions and cell zones).

You can manage your objects using several tools accessible with hotkeys, onscreen tool buttons, text

commands, or by using tools in the Manage Objects dialog box. Tools exist for operations such as

object creation, modification, changing propertes, alignment, remeshing, deleting, merging, and moving.

... Object Attributes

... Object Entities

... Managing Objects

Each object has attributes such as object type, cell zone type, and priority.

Object Type

The following object types are available:

Geometry

Objects imported through CAD using the CAD Faceting option (see Importing CAD Files (p. )) or

created for a given geometry.The geometry objects may be non-conformal.

Mesh

Objects that are good quality surface mesh representations of the geometry. Mesh objects may contain

multiple volumes with shared faces.They may be imported using the CFD Surface Mesh option for

CAD import or created using the object wrapping options. Mesh objects can also be created using

the Sew operation.

Cell Zone Type

The object cell zone type indicates the type of cell zone created when the mesh is generated based on

objects.

objects.

Figure . : Mesh With Different Cell Zone Types (p. ) shows a CutCell mesh with different cell

zone type assigned to respective objects.

Objects and Material Points

Figure . : Mesh With Different Cell Zone Types

Priority

The object priority controls the inclusion of the mesh entities. In case of overlapping objects, the entities

in the overlapped region will be included with the object having a higher priority value.

Figure . : Use of the Object Priority for Overlapping Objects (p. ) shows an example with over-

lapping objects. The overlapped region is included with the zone corresponding to the object

having the higher priority value (in this case, ).

Figure . : Use of the Object Priority for Overlapping Objects

Note

Multiple objects having the same priority assigned will be merged into a single cell

zone, irrespective of cell zone type.

Priority is also important when objects are created for bounding boxes or wind tunnels, and so

on. In such cases, the object created for a bounding box or wind tunnel must be assigned the

lowest priority.

Objects

.... Creating Objects

Figure . : Creating Objects—Example (p. ) shows the Subtract method for creating objects, using

an example with three non-intersecting bodies.

Figure . : Creating Objects—Example

The order of priority assigned to individual objects is important when using the Subtract method.

Zones in higher priority objects will be ignored when defining lower priority objects. In this case the

order of priority is object- > object- > object-.

Figure . : Objects Defined Using the Subtract Method

.

.

Select the face and edge zones comprising the innermost body, set the Cell Zone type, and set the

highest Priority value.

.

Select the face and edge zones comprising the inner body, set the Cell Zone type, and set an interme-

diate Priority value.

.

Select the face and edge zones comprising the outer body, set the Cell Zone type, and set the lowest

Priority value.

Note

Objects (defined or imported) are independent of each other; that is, objects do not share

face and/or edge zones. In cases where objects are defined using a common face/edge

zone, the common face/edge zones are duplicated to make the objects independent.

Object entities include face zone labels, volumetric regions, and cell zones. Volumetric regions and

cell zones are available only for mesh objects.

Face zone labels: For geometry objects, these are groups of face zones comprising the object. For mesh

object is created by merging multiple mesh objects, the face zone labels represent the objects that were

merged.They provide the link to the original geometry.

When the CAD Assemblies option is selected for CAD import, you can set up labels for the CAD

zones, if required. Named Selections are also imported as labels. These labels are preserved

throughout the object-based meshing workflow in Fluent Meshing.

Several tools for managing Face Zone Labels are available via the context-sensitive menus.

Note

Geometry objects can contain unlabeled zones. Mesh objects always contain face zone

Note

labels which are derived from the associated geometry objects. In case of unlabeled zones

in the geometry object, the mesh object face zone label is the same as the associated

geometry object.

Volumetric regions:These are finite, contiguous domains that are ready for volume meshing.

Cell zones:These are created when the volume mesh is generated.

.... Using Face Zone Labels

Various options are available for face zone labels via the context-sensitive menus in the tree:

The context-sensitive menu for Face Zone Labels contains options for drawing and selecting all labels

and obtaining an overall summary or detailed information about the face zone labels.

For Geometry Objects, you have these additional options:

– Unlabeled face zones can be labeled using the Create Labels... option.

The Create Labels dialog box opens. Select the face zones from the Face Zones selection

list and specify an appropriate Label Name. For geometry objects, you can choose to list

all available object face zones or only unlabeled object face zones for selection. Enable the

Objects

Create a label for each face zone checkbox to generate an individual label for each face

zone.

– Use the Remove All Labels from Zones... to remove labeled face zones from an object.

The Remove All Labels dialog box opens. Select the Object and Labeled Face Zones, and

then click Remove All.

Note

Unlabeled face zones are not supported for Mesh objects.

– Unlabeled zones can be drawn and/or selected without having to create a new label using the

Unlabeled Zones... options.

Note

For Mesh Objects, you have the additional Join/Intersect... option which opens a dialog box to

assist with creating a conformal surface mesh.

The context-sensitive menu for individual labels contains options for renaming, merging, and deleting

face zone labels in addition to the standard options for drawing and selecting all labels, and obtaining an

overall summary or detailed information.

You can also add or remove zones from an existing face zone label.

– Select Add Zones... from the context sensitive menu to open the Add Zones to Label dialog

box. Select the face zones and click Add. For geometry objects, you can add unlabeled zones or

those already included in other labels within the object selected.

– Select Remove Zones... from the context sensitive menu to open the Remove Zones from Label

dialog box. Select the face zones and click Remove.

For Mesh Objects, the context-sensitive menu for individual labels contains additional options for:

– connecting the face zones using Join/Intersect....

– finding and repairing face connectivity and quality problems using Diagnostics....

– creating or recovering periodic boundaries using Recover Periodic....

commands, or by using tools in the Manage Objects dialog box.

Tools exist for operations such as object creation, modification, changing propertes, alignment,

remeshing, deleting, merging, and moving.

.... Using hotkeys and onscreen tools

.... Using the Manage Objects Dialog Box

Tools for the most common object management operations are accessible via hotkeys, icons, or text

commands.

..... Creating Objects for CAD Entities

..... Creating Objects for Unreferenced Zones

..... Creating Multiple Objects

..... Easy Object Creation and Modification

..... Changing Object Properties

..... Automatic Alignment of Objects

..... Remeshing Geometry Objects

..... Creating Edge Zones

When the CAD Assemblies option is selected for CAD import, the CAD entities can be used to create

or modify geometry/mesh objects. The objects are associated with the CAD entities (which are then

locked), enabling re-importing or updating of selected parts or bodies using different faceting

qualities and topology representations for quick design changes and updates.

Use the options in the Object menu for CAD entities for creating geometry/mesh objects and modifying

existing objects. Select the CAD entities in the tree and then choose the appropriate menu option. Al-

ternatively, select the CAD objects in the graphics display and select the option from the CAD Tools. See

Creating and Modifying Geometry/Mesh Objects (p. ) for details.

Use the options in the CAD Association menu for geometry/mesh objects for modifying the selected

objects based on the associated CAD entities.You can also attach or detach the CAD entities from the

objects. See CAD Association (p. ) for details.

Use the options in the Create Objects dialog box to define objects for unreferenced boundary face

zones and edge zones. Right click Boundary Face Zones in the Unreferenced branch of the tree

and select Create New Objects... from the context-sensitive menu.

. Enter an appropriate name in the Object Name field.

You can also have the object name generated automatically by leaving the Object Name field

blank. In this case, the object name will be assigned based on the Prefix, cell zone type, and

priority specified (for example, an object named object-fluid:- has prefix object-, cell zone

type fluid, priority , and object ID ).

. Select the appropriate option from the Cell Zone Type drop-down list.

. Set the priority.

. Select the appropriate type from the Object Type drop-down list (default, geom).

. Enable the Create a label for each face zone checkbox to generate an individual label for each

face zone.

. Click Create.

Objects

You can also create one object per selected zone using the command /objects/create-mul-

tiple. This is particularly useful for CAD exported models, as you can define an object per part.

An object will be created for each selected zone and will be named automatically based on the

specified prefix and priority. The name assigned is prefix face zone name-priority:object ID. (For

example, an object named object-wall-: will be created for the face zone wall, with the specified

prefix object- and priority . The object ID is .)

. Specify the first and last zone for which objects are to be created.You can also use wild-cards for spe-

cifying the face zones to be considered.

Note

Note

You need to specify valid zone names or IDs.

. Specify the prefix to be used for the object name and the cell zone type.

. Specify the priority for the first object (for the first zone selected) and the increment in priority.

When the increment is set to a value greater than zero, the priority will be assigned in the order

of face zone ID. If the increment is set to zero, all objects will have the same priority.

A geometry object will be created for the first and last zone (as specified) and for all valid face zones

having IDs between the first and last zone.

You can easily move a zone from one object to another or create a new object using the Transfer

Zones tool (

) or Ctrl+Shift+Y hotkey combination.

. Select the zone(s) to be moved or to form a new object.

. Press the hotkey combination or click

.

. If a target object is set, the selected zone(s) are moved to the target. If no target is set, enter the

new object name in the Create Geometry Object dialog box.

To set a target object,

. Select the object using the mouse probe.

. Press the hotkey combination Ctrl+S or

.

Note

Empty objects will be automatically deleted.

Use the Change Object Properties dialog box to change the properties of objects based on selections

in the graphics window. Select one or more objects and then use the hot-key Ctrl+Shift+N  to open

the Change Object Properties dialog box.

Alternatively, select the objects in the Model tree and then select Rename/Change Properties...

from the menu available to access the Change Object Properties dialog box.

If a single object is selected, you can specify a new object name. If multiple objects are selected,

you can specify a common prefix for the objects selected. This enables you to easily view the objects

with the same prefix using the tree view button for selection lists. You can also choose to rename

object zones and set the geometry recovery option for the object zones (high or low).

You may also fit objects together in precise alignment, for example to position a flange on a body

by aligning bolt holes.

The procedure is initiated via the hotkey Ctrl+Shift+G, and uses a temporary local coordinate systems

(LCS) to achieve the alignment.

Defining a local coordinate system by selecting - nodes works as follows:

If only  node is selected, the LCS origin is at the node location and axes are aligned to global co-

ordinate system.

For  nodes, the LCS origin is at the midpoint of nodes and axes are aligned to global coordinate

system.

For  nodes, the origin is at the first point, the LCS x-axis is along a vector from the first to the second

point, and the LCS y-axis is along a vector from the first point to the 3rd point.

For ,  or  nodes, the first  points define a circle.The LCS origin is at the center of the circle and

the z-axis is normal to the circular plane (positive direction is determined by the right-hand rule).

– For  nodes, the x-axis is defined by a vector from the center of the circle to the projection of the

4th point on the circular plane.

mid-point of 4th and 5th points on the circular plane.

circumcenter of 4th, 5th and 6th points on the circular plane.

You can create mesh objects from the geometry objects without wrapping by using the Remesh

. Select Remesh... in the context-sensitive menu for geometry objects to open the Remesh dialog box.

. Select Individually or Collectively from the Target list.

Enter the object name when using the collective option.

Objects

. Click OK.

The size field based on currently defined sizing controls or size functions will be used to remesh

the geometry objects.

You can create edge zones on selected face zones or selected surfaces using the onscreen tools or

context menus. This feature is described in Extract Edge Zones (p. ).

The Manage Objects dialog box contains options that enable you to define objects and perform

certain object manipulation operations.

Right-click on Model in the tree and select Object Management... from the menu to access the

Manage Objects dialog box.

Select the Objects, Face Zones, or Edge Zones from their respective lists as required.

Note

If edge zones are to be included in the object definition, they must have been cre-

ated and visible in the lists.

List all zones controls how face and edge zones are listed.

– If enabled, all available zones are listed.

– If disabled, the lists will contain only zones that are not included in existing objects.You can use

this to identify zones that are not associated with objects.

Select Object Zones controls highlighting of face and edge zones in the lists. If enabled, when an

object is selected, face and edge zones in the object will be highlighted.

Choose one of the tabs to access the object management tools.

..... Defining Objects

..... Object Manipulation Operations

..... Object Transformation Operations

You can define the objects using the options in the Definition tab of the Manage Objects dialog

box.

.

Enter an appropriate name in the Object Name field.

.

Select the appropriate option from the Cell Zone Type drop-down list.

.

Set the priority.

.

Select the appropriate type from the Object Type drop-down list (default, geom).

.

Click Create.

You can modify the object definition using the Change option in the Manage Objects dialog box.

Select the object to be modified, make the necessary changes in the Definition tab, and click Change.

You can also use the Change Type to Mesh option in the menu available for geometry objects.

Objects can be deleted using the Delete option in the Definition tab. You can also enable Include

Faces and Edges to delete the faces and edges comprising the object, when the object is deleted.

Note

When an object is deleted along with the face and edge zones comprising the object,

any corresponding face/edge groups will also be deleted.

The following object manipulation operations can be performed using the options in the Operations

tab of the Manage Objects dialog box or using the options from the menu available on any geometry

or mesh object selected in the Outline View:

Objects of the same type (geometry or mesh) can be merged using the Merge Objects... option. Specify

the name for the merged object in the Merge Objects dialog box.

When multiple mesh objects are merged, the face zone labels represent the objects that were

merged.

Important

Merging zones that have different face zone labels will result in a merged zone with

the original labels appended.

Wall face zones comprising objects can be merged using the Merge Walls option.

The edge zones comprising an object can be merged into a single edge zone using the Merge Edges

option.

Note

If the object contains edge zones of different types (boundary and interior), the edge

zones of the same type (boundary or interior) will be merged into a single edge zone.

Intersection loops can be created within an object or between objects using the options in the Intersection

Loops group box.

Objects

Edge zones can be extracted from the face zones included in the specified objects, based on the feature

Objects

angle value specified using the options in the Edge Zones group box.You can specify whether only

feature edges or all edges are to be extracted for the objects selected. Previously created edges will

automatically be disassociated from the object and added to the Unreferenced branch of the Outline

View tree.

Note

– This functionality is also available in the Extract Edges dialog box. See Extract Edge

Zones (p. )

– Similar functionality is also available in the Feature Modify dialog box and Surface Retrian-

gularization dialog box. See Creating and Modifying Features (p. ) and Remeshing

Boundary Zones (p. ).

A face group and an edge group comprising the face zones and edge zones included in the specified

objects can be created using the options in the Zone Group group box.

The face zones comprising the object can be separated based on the angle or seed specified using the

options in the Separate Faces group box.

When the face zones and/or edge zones comprising an object are deleted, you will be prompted to update

the object definition.You can use the command /objects/update to update the defined objects

per the changes.

You can rename the face and edge zones comprising the object based on the object name and also

specify the separator to be used.

The following object transformation operations can be performed using the options available in the

Transformations tab of the Manage Objects dialog box:

Objects can be rotated using the Rotate option. Specify the angle of rotation and the pivot point and

the axis of rotation by selecting - nodes in the graphics window.

The pivot point and the axis of rotation can be defined by selecting - nodes as follows:

– For  nodes, the pivot point is at the midpoint of the nodes selected and the axis of rotation

is the global z-axis.

– For  nodes, the pivot point is at the first node selected. The axis of rotation is the local z-axis

normal to the plane defined by the three points, the positive direction is determined by the

right-hand rule.

– For ,  or  nodes, the first  points define a circle. The pivot point is at the center of the circle.

The axis of rotation is the local z-axis normal to the circular plane, the positive direction is de-

termined by the right-hand rule.

Objects can be scaled using the Scale option. Specify the scale factors (X,Y, Z) for the scaling operation.

Objects can be translated using the Translate option. Specify the vector components to define the

translation, or click Define and select two screen locations to determine the translation.

In addition to objects, material points can be defined to allow the mesher to separate the cell zone.

Typically, a material point can be defined to retrieve a cell zone for which an object cannot be defined,

or the object definition alone is not sufficient to retrieve the cell zone. Material points can also be used

to retrieve regions from a non-contiguous cell zone. Contiguous regions will be separated based on

the respective material points defined. The cell zone retrieved based on the defined material point will

be of the type fluid and have the specified name.

The following examples demonstrate the use of a material point in addition to objects:

Some cases involving “dirty” geometry may result in multiple voids. In this case, the volume to be meshed

can be recovered by defining an object comprising the zones enclosing the domain to be meshed, combined

with a material point within the expected meshed domain (see Figure . : Using Material Points—Ex-

ample (p. )).

Figure . : Using Material Points—Example

Note

The intersection loops can be created (see Object Manipulation Operations (p. )) to re-

cover the intersecting features accurately.

In Figure . : Example—CutCell Mesh, Only Objects Defined (p. ), the use of only objects to define the

meshed domain results in a mesh with two cell zones, solid and fluid.

Material Points

Figure . : Example—CutCell Mesh, Only Objects Defined

By specifying a material point in addition to the object definition (fluid or dead), the fluid zone in

Figure . : Example—CutCell Mesh, Only Objects Defined (p. ) will be further separated into a fluid

zone (containing the material point) and a dead zone (see Figure (A) (p. )). If auto-delete-

dead-zones? is enabled (default), the separated dead zones will be deleted automatically (Figure

(B) (p. )).

(A) CutCell Mesh—Material Point and Objects Defined, auto-delete-dead-zones? Disabled

(B) CutCell Mesh—Material Point and Objects Defined, auto-delete-dead-zones? Enabled

Note

Note

For cases where a single region is separated by a double-sided surface (fan, radiator, or

porous-jump), you need to define a material point for each of the regions to be recovered

(that is, both upstream and downstream of the double-sided surface). Separate cell zones

will be recovered for each region on either side of the double-sided surface.

You can merge the cell zones manually after the mesh has been generated.

Figure . : Example—Fluid Surface Extracted From Geometry Objects and Material Point (p. ) shows the

use of a material point in addition to objects defined to extract the internal fluid surface, using the object

wrapping operation.

Figure . : Example—Fluid Surface Extracted From Geometry Objects and Material Point

... Creating Material Points

Right-click Model in the tree and select Material Points... from the menu to access the Material

Points dialog box.

Click Create... to open the Create Material Point dialog box. Follow the process described.

.

Select the appropriate zones or objects in the graphics window.The selections should be such that the

material point created will lie at a central point in the fluid domain.

.

Click Compute to obtain the material point coordinates based on the selections.

You can also specify the coordinates manually if the material point location is known.

.

Enable Preview to verify that the location is appropriate.

.

Enter an appropriate fluid zone name in the Name field.

.

Use the List button to display the x-, y-, and z- coordinates of the selected material point(s) in the

console.

Use the Delete button to remove the selected material point(s).

.

console.

Use the Draw button to display the selected material point(s) in the graphics window.

Chapter : Object-Based Surface Meshing

Object-based meshing is the recommended meshing approach with which you can generate a tetrahedral,

hexcore, or polyhedral volume mesh, with or without inflation layers. In this approach, you first create

a conformal, connected surface mesh on all the objects to be meshed. The surface mesh, and material

points if required, are then used to identify the regions to be filled with the volume mesh.

This chapter describes the processes used to create a conformal, connected surface mesh. Steps to

create the volume mesh are described in Object-Based Volume Meshing (p. ). Refer to Objects and

Material Points (p. ) for more information on meshing objects.

Important

Ensure that the model is suitably scaled during import and the global minimum size is at

least . to avoid numerical problems during mesh generation.

The tools to complete the object-based surface meshing steps are found in the context-sensitive menus

in the Outline View or in the onscreen tools and hotkeys. Instructions are described in the following

sections.

.. Surface Mesh Processes

.. Preparing the Geometry

.. Diagnostic Tools

.. Connecting Objects

.. Advanced Options

In principal, there are two basic workflows to create a conformal, connected surface mesh from an un-

connected assembly.

Note

It is assumed that objects are already created upon CAD import. Object management,

if necessary, is described in Objects (p. ).

Note

Single fluid volume using Wrapper based workflow

The basic Wrapper based workflow for a single fluid volume simulation follows these steps:

. Import the CAD model using the CAD Faceting tessellation option.

Geometry objects are created. See Importing CAD Files (p. ) for additional information.

. Define sizing and compute the size field.

Scoped Sizing is recommended to apply individual size controls on specific objects as required.

See Defining Scoped Sizing Controls (p. ) for additional information.

. Define material points to assist in identifying the fluid volume.

See Material Points (p. ) for additional information.

. Check and fix the geometry, particularly gaps.

You can use the context menu Diagnostics → Geometry, accessible from any Geometry object,

to assist in finding any geometry issues. See Diagnostic Tools (p. ) for additional information.

Missing geometry objects may be constructed as described in Preparing the Geometry (p. ).

. Define periodic boundaries, if applicable.

See Creating Periodic Boundaries (p. ) for additional information.

. Wrap the model.

Step through the options available in the Wrap context menu. See The Wrapping Process  (p. )

. Check the mesh and improve the quality, if necessary.

You can use the context menu Diagnostics → Connectivity and Quality, accessible from any

mesh object.

Complex topology using Join and Intersect based workflow

The basic Join/intersect based workflow for complex topology such as CHT simulation, follow these

steps:

. Import the CAD model using the CFD Surface Mesh tesselation option.

steps:

Mesh objects are created. See Importing CAD Files (p. ) for additional information.

Note

If the assembly has already been connected (for example, using Share Topology

operations in ANSYS DesignModeler or SpaceClaim), it is sufficient to just import the

CAD using the One object per file and CFD Surface Mesh options.

. Check the mesh and fix the connectivity, if necessary.

Object-Based Surface Meshing

. Merge all objects to a single object using the Merge option in the context menu.

. Connect all bodies.

You can use the Join/Intersect context menu or the onscreen tools for Join or Intersect. See

Connecting Objects (p. ) for additional information.

. Optionally define sizing, compute the size field and remesh if necessary.

Remesh is recommended as it often reduces mesh count and improves quality while maintaining

sufficient mesh density. You can use the Remesh Faces context menu or the onscreen tools.

Computing a size field is necessary only if you choose to remesh. Scoped Sizing is recommended

to apply individual size controls on specific objects as required. See Defining Scoped Sizing

Controls (p. ) for additional information.

When the surface mesh is conformally connected and of sufficient quality, proceed to generate the

volume mesh as described in Object-Based Volume Meshing (p. ).

When the geometry is imported from CAD, there may be a number of gaps and the faceted geometry

may be disconnected. Though operations such as merging nodes and faceted stitching can be used to

partially connect the model, some gaps may remain and features may be lost.

You may want to perform tasks such as create a wind tunnel or far-field domain, close annular gaps,

create capping surfaces for inlets or outlets, or create groups of zones for models with a large number

of zones. Right-click on Model in the tree and select the appropriate option from the menu to access

the options to perform such operations.

... Using a Bounding Box

... Closing Annular Gaps in the Geometry

... Patching Tools

... Using User-Defined Groups

The bounding box tool can be used to create a wind tunnel or far-field domain for the imported

geometry. A geometry object can be created for the bounding box surface created. You can also use

the bounding box tool to create a body of influence to be used for defining size functions. See Using

the Bounding Box Dialog Box (p. ) for details on the options for creating a bounding box. Right-click

on Model in the tree and select Construction Geometry → Bounding Box... to open the Bounding

Box dialog box.

Preparing the Geometry

See Creating a Cylinder/Frustum (p. ) to create a cylindrical or annular surface to close radial gaps

in the geometry. A geometry object can be created for the surface created. Right-click on Model in

the tree and select Construction Geometry → Cylinder... to open the Cylinder dialog box.

Figure . : Closing a Radial Gap (p. ) shows an example where a radial gap is closed using a cyl-

indrical surface.

Figure . : Closing a Radial Gap

.

Select  Arc,  Height Node in the Options list.

.

Click Select Nodes... and select  nodes on one circle and one (height node) on the other across the

radial gap.

.

Enter an appropriate value for Edge Length.

.

Enable Create Object and disable Caps.

.

The patching tools enable filling of unwanted holes in the geometry. A hole may be bounded by either

free edges or feature edges. Use the patching tools to:

patch holes associated with free faces in multiple zones

fill punched holes in a single zone

cap inlets/outlets and assign the appropriate zone type

patch other complex shapes to close gaps including sharp angles and small pockets in the geometry using

the loop selection tools

Use the patching tools to locate and fix the major holes in the geometry. If you miss any holes, you

can fix them later using the hole detection feature. See Fixing Holes in Objects (p. ) for details.

.... Using the Patch Options Dialog Box

.... Using the Loop Selection Tool

When the patching tools are used, by default, the new faces are added to a new face zone and are

remeshed. These options are available in the Patch Options group in the ribbon.

Remesh enables the automatic remeshing of the patched area.

Separate enables the creation of a separate face zone/object for the new faces created. Additional options

for object/zone granularity and type are available in the Patch Options dialog box.

The Patch Options dialog box contains options for object/zone granularity and type and is available

when the Separate option is selected. Specify the object/zone granularity as follows:

Select New Object to create a new object for the face zones. Specify the object name and a label name.

If the label name is not specified, the object name will be used as the label name. Face zone names will

be the same as the label names. Select the Object Type and Zone Type from the lists.

Select Add to Object to add the face zones to an existing object. Select the object and specify a label

name. If the label name is not specified, the default name patch:# (# indicates the ID) will be used. Face

zone names will be the same as the label names. Select the Zone Type from the list.

Select Add to Unreferenced to create unreferenced face zones. Select the Zone Type from the list.The

default name patch:# (# indicates the ID) will be used for the zone name.These zones will be available

in the Unreferenced branch of the tree.

Using Edge/Node Selections

Select edges/nodes in the graphics window to fix the holes in the geometry.

Fixing holes by selecting edges.

.

.

Set the patching options in the Patch Options group in the ribbon.

.

Select the edge filter (

or hot-key Ctrl+E) and select any edge on the hole boundary.You can

select either free edges or feature edges.

.

Click

or press F5 to create the surface that closes the hole.

a.

If the Separate option is enabled, set the object/zone granularity and type in the Patch Options

dialog box (Using the Patch Options Dialog Box (p. )). If the Remesh option is enabled, the

face zones will be remeshed.

b.

Click Create in the Patch Options dialog box.

Figure . : Creating a Surface Using an Edge (p. ) shows an example where the capping surface

is created by selecting an edge on the existing object.

Figure . : Creating a Surface Using an Edge

Fixing holes by selecting nodes.

.

.

Select the node filter (

or hot-key Ctrl+N) and select the nodes around the hole.

.

Press

or F5 to create the surface that closes the hole.

a.

b.

Figure . : Creating a Surface Using Nodes (p. ) shows an example where the capping surfaces

are created by selecting nodes on the existing object.

Figure . : Creating a Surface Using Nodes

Patching Multiple Holes in a Single Zone

All holes associated with free edges or punched holes in a single zone can be closed in a single

patching operation using the hot-key Ctrl+R (

).

.

.

Select the appropriate entity for the operation:

For patching holes with free faces, select the appropriate face zones in the graphics window.

For patching punched holes, select a face adjacent to a hole in the face zone.

Note

Punched holes can be closed only in a single face zone having finite thickness.

There should be no free faces in the face zone being patched.

.

Click

or use the hot-key Ctrl+R.

a.

dialog box (Using the Patch Options Dialog Box (p. )). If the Remesh option is enabled, the face

zones will be remeshed.

b.

The loop selection tool can be accessed by clicking

in the graphics window or using the hot-

key Ctrl+Shift+L. This tool provides additional options, such as using fewer node selections, for cre-

ating the capping surface. You can also select positions to define the loop.

The following selection options are available:

In the first group of tools, choose how the path between selected nodes/positions is defined - by edges,

feature, boundary, or direct path. Click

to switch between selecting nodes or positions to define the

loop.

The second group of icons is used to select open or closed loop.Then, for closed loop mode, you can

loop.

choose how the path between the first and last nodes is defined - by edges, feature, boundary, or direct

path.

After making the necessary selections, click

or use the hot-key Ctrl+K in the Loop Selection

mode to open the Create Cap dialog box.

The Create Cap dialog box contains options for object/zone granularity and type and for remeshing

the capping surface.

.

Specify the object/zone granularity.

Select New Object to create a new object for the face zones. Specify the object name and a label

name. If the label name is not specified, the object name will be used as the label name. Face zone

names will be the same as the label names. Select the Object Type and Zone Type from the lists.

name. If the label name is not specified, the default name patch:# (# indicates the ID) will be used.

Face zone names will be the same as the label names. Select the Zone Type from the list.

Select Add to Unreferenced to create unreferenced face zones. Select the Zone Type from the list.

The default name patch:# (# indicates the ID) will be used for the zone name.These zones will be

available in the Unreferenced branch of the tree.

.

Enable Remesh to remesh the capping surface created.

.

Click Create in the Create Cap dialog box.

For the list of hot-keys associated with the options in the Loop Selection toolbar, refer to Ap-

pendix C: Shortcut Keys (p. ).

You can define user-defined groups to better handle large models. The options for manipulating user-

defined groups are available in the User Defined Groups dialog box. Right-click on Model in the tree

and select Groups... to open the User Defined Groups dialog box.

You can create a face group and an edge group comprising the face zones and edge zones included

in the specified objects using the options in the Zone Group group box in the Operations tab in the

Manage Objects dialog box. You can activate a particular group using the Activate option in the User

Defined Groups dialog box.

Additionally, a face zone group is automatically created when a mesh object is created using the Sew

operation. This face zone group is prefixed by _mesh_group, and enables easy selection of mesh object

face zones for various operations (improve, smooth, and so on).

Note

When an object is deleted along with the face and edge zones comprising the object, the

corresponding groups will also be deleted.

Important

You cannot create a new group having the name global, or having the same name as one

of the default groups.

The options in the Diagnostic Tools dialog box enable you to find and fix problems in boundary meshes,

or display boundary mesh statistics, of selected objects. The Diagnostic Tools dialog box is accessed

by selecting the appropriate option from the Diagnostics sub-menu available by right-clicking on any

geometry or mesh object selected in the Outline View.

Diagnostic tools are available for the following:

finding and fixing Geometry problems, such as gaps or intersections between objects.

finding and fixing Connectivity problems in the surface mesh, such as free or multi-connected edges,

and overlapping or intersecting faces.

finding and fixing Quality problems in the surface mesh.

A Summary table of mesh statistics can be obtained using the Summary button at the bottom of the

Diagnostic Tools dialog box, or from the context-sensitive menu on any geometry or mesh object se-

lected in the tree.

... Geometry Issues

... Face Connectivity Issues

... Quality Checking

Diagnostic Tools

... Summary

Note

When selecting Diagnostics... from under a mesh object’s Face Zone Label, the Geometry

options are not available. The dialog box contains only Face Connectivity and Quality options

for the boundary zones included in the Face Zone Label.

Problems in the geometry, such as gaps or intersections can be located and fixed using the diagnostic

tools. Select the objects (geometry or mesh) in the Model tree, and then select Geometry... from the

Diagnostics sub-menu available from the context-sensitive menu.

.

Select the desired Issue and then set the relevant marking options.The issues that can be diagnosed

are as follows:

Self Intersections

Cross Intersections

Self Face Proximity

Cross Face Proximity

Self Edge Proximity

.

Click Mark to identify and obtain a count of the Unvisited problems in your boundary mesh.

.

Click First (Next) to step through the problems individually. At each step, the identified problem region

will be highlighted in the graphics window.

.

.

.

To correct the identified problem (if necessary), click the appropriate button in the Operations group

box.You can choose to fix all identified problem areas or the area that is currently displayed.

Note

Many other geometry modification tools are available. The buttons presented in the Oper-

ations group box represent the most likely tools for the type of issue.

Problems in the surface mesh such as free or multi-connected faces, self-intersecting faces, or other

problematic configurations can be located and fixed using the diagnostic tools. Select the objects

(geometry or mesh) in the Model tree, and then select Connectivity and Quality... from the Diagnostics

sub-menu available from the context-sensitive menu.

Note

If a Face Zone Label is selected under a mesh object, the Diagnostics... menu will not

have any submenu choices, but will open directly with Face Connectivity and Quality

options available.

.

Select the boundary zones to be examined.

Select All to select the boundary zones from a list including all boundary face zones available.

Select Unmeshed to select the boundary zones from a list of the unmeshed tri zones available.The

unmeshed zones are those that are not connected to a volume mesh.

.

On the Face Connectivity tab, select the desired Issue and then set the relevant marking options.The

issues that can be diagnosed are as follows:

Free

Multi

Self Proximity

Duplicate

Spikes

Islands

Steps

Slivers

Point Contacts

Invalid Normals

Note

Free

Multi

Duplicate

Spikes

Islands

Steps

Slivers

Note

Zone-specific or scoped prism settings should be applied prior to using this option.

Leaks

Deviation

.

.

.

Note

Many other mesh modification tools are available. For example, you can do Local Remesh

(use the hotkey Ctrl+Shift+R) or Smooth (F6) instead of Collapse (Ctrl+J) to remove slivers.

The buttons presented in the Operations group box represent the most likely tools for the

type of issue.

Problems with the surface mesh quality can be located and fixed using the diagnostic tools. Select the

objects (geometry or mesh) in the Model tree, and then select Connectivity and Quality... from the

Note

have any submenu choices, but will open directly with Face Connectivity and Quality tabs

available.

.

.

On the Quality tab, set the number of quality measures and specify up to three quality measures to be

used.Then select from the following quality measure options.

Skewness

Size Change

Edge Ratio

Area

Aspect Ratio

Warp

Dihedral Angle

Ortho Skew

.

.

.

To correct the identified problem (if necessary), select the appropriate option in the Operations group

box and click Apply for All. Alternatively, you can choose to collapse or smooth all marked faces that

are currently displayed.

For more information on how Fluent calculates the quality and adjusts the mesh, see the Quality

Measures (p. ) page.

Note

(use the hotkey Ctrl+Shift+R) instead of Smooth (F6) or Collapse (Ctrl+J) to remove a

skewed face. The buttons presented in the Operations group box represent the most likely

tools for the type of issue.

A tabular summary of mesh statistics can be displayed in the console by selecting Summary from the

context sensitive menu for a geometry or mesh object in the Outline View tree.

The displayed data includes the number of free-, multi-, and duplicate faces; face quality (skewness)

statistics, and total number of faces and face zones. This is the same information as is displayed by

clicking the Summary button in the Diagnostic Tools dialog box.

The join and intersect operations are used to connect face zone labels within a mesh object by joining

overlapping faces or intersecting face zones. In case of multiple mesh objects, merge the objects into

a single mesh object and then proceed to join/intersect them. For best results, it is recommended that

faces be of similar size where the join or intersect operation is occurring. The process is interactive, fast,

scriptable, and enables direct control over local shape and quality, and volumetric and surface overlaps.

Join/Intersect may be employed as a bottom-up strategy that enables you to build multiple sub-assem-

blies individually, and then connect the sub-assemblies to create the final assembly. It can be used to

connect all the face zone labels within a mesh object into the final assembly in one operation. Support

for part replacement without global remeshing is inherent in the process.

An example of the join operation is shown in Figure . : Overlapping Surfaces (p. ) and Fig-

ure . : Connected Surfaces After Join (p. ). The overlapping area of the face zones is separated

based on the parameters specified and merged into a single separated face zone after the join operation.

The joined surfaces will be locally remeshed. The multi-connected faces indicate that the zones are now

connected.

Connecting Objects

Figure . : Overlapping Surfaces

Figure . : Connected Surfaces After Join

An example of the intersect operation is shown in Figure . : Intersecting Surfaces (p. ) and Fig-

ure . : Connected Surfaces After Intersect (p. ). The intersecting faces are marked based on the

parameters specified. The intersecting face zones are connected and locally remeshed.

Figure . : Intersecting Surfaces

Figure . : Connected Surfaces After Intersect

Important

After any Join or Intersect operation, remesh is called automatically. To disable the post-

remesh operation, use one of the text commands:

/objects/join-intersect/controls/remesh-post-intersection?

no

/boundary/remesh/controls/intersect/remesh-post-intersection?

no

The following options are available for connecting object zones:

... Using the Join/Intersect Dialog Box

... Using the Join Dialog Box

... Using the Intersect Dialog Box

The Join/Intersect dialog box is accessed from the context-sensitive menu under any Mesh Object,

or any Face Zone Labels under a Mesh Object. For best results, the following practices are highly

recommended:

Prepare clean input prior to using Join/Intersect:

– Resolve free, duplicate and sliver faces using the Diagnostics tools. See Diagnostic Tools (p. ).

– Identify self-proximity locations and separate it into different zones using the Diagnostics tools.

– Remove gaps between the face zones to be joined to get clean contacts (overlaps). Alternatively, choose

Absolute Tolerance with a value greater than or equal to the known gap if joining over smaller gaps.

– Have similar mesh sizes (density) on face zones to be joined.

If wrapped meshes are used with Join, use the High option together with a scaled Size Function to produce

a very fine mesh. After join, all the surfaces may be remeshed with the default size function.

The Join/Intersect dialog box can be used as follows:

.

Select Join/Intersect... from the context-sensitive menu available for the Mesh Object selected in the

tree to open the Join/Intersect dialog box.The corresponding Face Zone Labels and Face Zones are

listed.

Note

Face Zone Label represents either the collective name of the face zones in the mesh

object or, in the case of conformal faceted import with one object per part, the bodies

of the part.

.

Choose Join or Intersect in the Operation group box.

Tip

Always use the join operation first, then intersect.

a.

For the Join operation, Skip Bad Joins is enabled by default (in the Controls group box).

b.

Specify an appropriate value forMin. Dihedral Angle.

The Skip Bad Joins option enables joined pairs to be undone locally if a self intersection is

found or if the smallest dihedral angle is less than the specified value.

.

In the Parameters group box, specify the decision thresholds for Angle (default is  degrees) and

Tolerance (default is relative tolerance of ., or % of local triangle size).

Check Absolute Tolerance to specify tolerance is in the same dimensional units as the geometry.

.

Use the global Join (Intersect), under the Face Zones list, to perform the selected Operation on selected

.

Face Zones using the specified Parameters.

Alternatively, use Local controls to perform the operations on pairs of overlapping or intersecting

face zones.

Local is recommended for geometry where you do not know the tolerances.

Note

Length scales of geometric features should be smaller than the local triangle size.

a.

Click Find Pairs in the Local group box.

b.

Click First (and subsequently Next) to step through each pair of surfaces individually.The display

is automatically limited to the area of overlap/intersection since Bounded View is enabled by default.

c.

Click Mark Faces to view the overlapping/intersecting faces.

d.

Click Join (or Intersect) in the Local group box to perform the selected Operation on the selected

pair of surfaces.

Important

Since the join operation separates the two overlapping face zones and keeps only one

separated face zone, it is possible that the separated zone may overlap with a third zone,

so you should repeat the operation iteratively until no overlaps are found.The intersection

operation does not separate the face zones; still, it is a good practice to repeat the operation

iteratively until no intersections are found.

The surface should be inspected for self-intersections, duplicates, and so on after Join or

Intersect operations using the Diagnostics tools.

Important

Quads are not supported by Join or Intersect.

Use the Join dialog box to join overlapping face zones based on selections in the graphics window.

.

Select the overlapping face zones in the graphics window and click

. Alternatively, use the hot-key

.

Ctrl+T to invoke the miscellaneous tools and then Ctrl+J to open the Join dialog box.

.

Specify an appropriate Tolerance (default is relative tolerance of ., or % of local size). Alternatively,

enable Absolute Tolerance and specify a value greater than or equal to the known gap.

.

Click Mark. After verifying the marked faces, select the face zones to be joined again.

.

Click Join.

Click Undo if the results of the join operation are unsatisfactory. The operation can be undone

until the next mesh operation or until the Join dialog box is closed.

Use the Intersect dialog box to intersect face zones based on selections in the graphics window.

.

Select the intersecting face zones in the graphics window and click

Ctrl+T and then Ctrl+I to open the Intersect dialog box.

.

enable Absolute Tolerance and specify the absolute value.

.

Enable Separate if you need to separate the intersecting zones at the edge loop of intersection.

.

Retain the default selection of Ignore Parallel Faces and enter an appropriate value for Parallel Angle.

The default value is .

.

Click Mark. After verifying the marked faces, select the face zones to be intersected again.

.

Click Intersect.

Click Undo if the results of the intersect operation are unsatisfactory. The operation can be undone

until the next mesh operation or until the Intersect dialog box is closed.

Objects define the domain to be meshed. The following advanced options are available:

... Object Management

... Removing Gaps Between Mesh Objects

... Removing Thickness in Mesh Objects

... Sewing Objects

The Manage Objects dialog box contains the following tabs:

Definition: Used to create, modify, or delete objects.

Operations: Used for manipulations such as merge, extract edges, create groups, and separate faces.

Transformations: Used to rotate, scale or translate objects.

Manage Objects dialog box.See Using the Manage Objects Dialog Box (p. ).

Note

When the face zones and/or edge zones comprising an object are deleted, the object

definition will be updated. If all the zones associated with an object are deleted, the empty

object will be deleted as well.

Gaps between mesh objects can be removed using the options in the Remove Gaps dialog box. The

gaps can be between surfaces (face-face) or between a surface and an edge (face-edge).

.

Right click on the object in the Outline View. Select Advanced → Remove Gaps... from the context

sensitive menu.

.

Select Remove Gaps Between Objects in the Operation list.

.

Specify an appropriate value for the Min. Gap Distance, Max. Gap Distance, and Percentage Margin.

.

Specify an appropriate value for Critical Angle.The critical angle is the maximum angle between the

faces constituting the gap to be removed.

.

Ignore Orientation is enabled by default. If the thickness of any of the object selected is less than the

.

Max. Gap Distance, then you can disable Ignore Orientation. In this case the orientations of the normals

will be considered. Ensure that, the normals in the gaps to be removed are appropriately oriented (Fig-

ure . : Orientation of Normals in Gap (p. )).

Figure . : Orientation of Normals in Gap

.

Select the appropriate option for feature edge extraction (none, feature, or all) and specify the Extract

Angle to be used.

.

Select the type of gap in the Gap Type list (Face-Face or Edge-Face).

Advanced Options

For face-face gap removal, select the appropriate option for projection in the Order list.You can

choose to project the faces to the object of higher priority (Low To High Priority) or to the object

of lower priority (High to Low Priority).

.

Click Mark to see the faces marked for projection.

.

Click Remove to remove the gaps between the objects selected.

Figure . : Removing Gaps Between Objects—Face-Face Option (p. ) shows an example where a

face-face gap between mesh objects has been removed.

Figure . : Removing Gaps Between Objects—Face-Face Option

Figure . : Removing Gaps Between Objects—Face-Edge Option (p. ) shows an example where a

face-edge gap between mesh objects has been removed.

Figure . : Removing Gaps Between Objects—Face-Edge Option

The thickness across a mesh object can be removed by projecting the close surfaces to a mid-surface.

During the thickness removal operation, the object face zones will be separated in order to project

the close surfaces to the mid-surface and the separated zones will be merged back after the projection.

The options for thickness removal are available in the Remove Gaps dialog box.

Configurations can be distinguished as gaps or thicknesses based on the orientation of the normals

on the mesh object (Figure . : Gap and Thickness Configurations (p. )). The normals across a gap

configuration point toward each other, while for a thickness configuration, the normals point away

from each other.

Figure . : Gap and Thickness Configurations

When using the option for thickness removal, ensure that the object normals are appropriately oriented

depending on the configurations to be removed (see Figure . : Gap and Thickness Configura-

tions (p. )).

The generic procedure for removing thickness in objects using the Remove Gaps dialog box is as

follows:

.

.

Select Remove Thickness In Objects in the Operation list.

.

Specify an appropriate value for the Max. Gap Distance and Percentage Margin.

.

faces constituting the thickness to be removed.

.

.

Click Remove to remove the thickness in the objects selected.

Note

The thickness removal operation involves separation and merging back of face zones,

which may affect the mesh quality. It is recommended that you save the mesh before

proceeding.

Figure . : Removing Thickness in Objects (p. ) shows an example where the thickness in the

mesh object has been removed.

Figure . : Removing Thickness in Objects

The sewing operation is a face connecting operation applicable to mesh objects. Disconnected assem-

blies can be connected to create the conformal, triangular surface mesh on the specified objects. This

operation creates conformal mesh between bodies and produces a topology-verified model. Normals

are also reoriented suitably for further prism meshing.

The procedure to Sew objects is:

.

Select the mesh objects in the Outline View. Right-click and select Advanced → Sew... from the context

.

Ensure that the mesh objects for the sew operation are selected in the Objects list in the Sew dialog

box.

.

Specify the name for the mesh object to be created for the selected mesh objects.

.

If desired, disable the Improve option.

If disabled, you may need to improve the surface mesh quality of the mesh object created using

the options in the Diagnostic Tools dialog box and the Improve dialog box.

Figure . : Mesh Objects to be Connected (p. ) shows an example with disconnected mesh objects.

The sewing operation creates the conformal surface mesh by connecting the individual objects into

a single mesh object (Figure . : Mesh Object Created by Sewing (p. )).

Figure . : Mesh Objects to be Connected

Figure . : Mesh Object Created by Sewing

A face zone group is automatically created for the mesh object created by the Sew operation. This

face zone group is prefixed by _mesh_group, and enables easy selection of mesh object face zones

for various operations (improve, smooth, and so on).

Note

The sew operation is not needed for a single mesh object, or flow volume (only) extraction

type problems. You can use the options in the Diagnostic Tools dialog box and then use

the Improve dialog box or the command /objects/improve-object-quality to

improve the surface mesh (see Improving the Mesh Objects (p. )).

You can use the command /objects/sew/sew to connect the mesh objects. Specify the objects

to be connected and the name for the mesh object to be created.

.... Resolving Thin Regions

Surfaces in close proximity constitute thin regions in the mesh. Examples of thin regions include sharp

corners, trailing edge configurations, and so on, which may not be recovered accurately enough

during the sewing operation and surface elements may span between nodes on the proximal surfaces.

You can use the command /objects/sew/set/include-thin-cut-edges-and-faces to

allow better recovery of such configurations during the sewing operation.

.... Processing Slits

In cases containing baffles, when the shrink-wrap method is used for the object wrapping operation,

the mesh object is created with nearly overlapping surfaces representing the baffle. Though the surfaces

are nearly overlapping, there is a numerically a small angle between them (parallel face angle). Such

configurations constitute slits in the mesh object.

The command /objects/sew/set/process-slits-as-baffles? enables you to collapse

the nearly overlapping surfaces corresponding to the baffle when the sew operation is performed to

create the mesh object. Specify the maximum slit thickness relative to the minimum size specified

and the parallel face angle between the faces comprising the slit when process-slits-as-

baffles is enabled.

Note

When process-slits-as-baffles is enabled for the Sew operation, it is recommen-

ded that you check the mesh object created for voids or pockets. Use the command

/objects/merge-voids to remove any voids or pockets created in the mesh object

(see Removing Voids (p. ) for details).

.... Removing Voids

The command /objects/merge-voids enables you to remove voids or pockets created in the

Chapter : Object-Based Volume Meshing

This chapter describes the volume meshing approach with which you can generate a tetrahedral, hexcore,

polyhedral, or hybrid volume mesh, with or without inflation layers, for mesh objects created from the

imported geometry. You need to create a conformally connected surface mesh using the object wrapping

or join/intersect operations before generating the volume mesh. See Object-Based Surface Meshing (p. )

The tools to complete these steps can be found in the context-sensitive menus in the Outline View

tree. Instructions are described in the following sections.

..Volume Mesh Process

..Volumetric Region Management

.. Generating the Volume Mesh

.. Cell Zone Options

As an alternative, you can use the CutCell mesher to directly create a hex-dominant volume mesh for

the geometry based on meshing objects created. See Generating the CutCell Mesh (p. ) for details.

When the conformal, connected surface mesh is ready, use the Outline View tree to navigate the volume

meshing workflow as follows:

.

Set up Volumetric Regions.

Volumetric regions are finite, contiguous domains ready to receive a volume mesh. You use the

Compute menu option to initialize the volumetric regions within a mesh object. If you perform

operations such as merging or deleting, you should Validate the regions before computing the

volume mesh. The Update option will recompute existing volumetric regions while preserving

names and types.

Tools to compute, update and validate the volumetric regions, as well as tools to modify selected

regions, are accessible via the context-sensitive menus. For a full description of available operations,

see Volumetric Region Management (p. ).

.

Fill the volumetric regions collectively or individually, as appropriate.

a.

Right-click on any individual volumetric region and you can access menus to setup Scoped Prism,

Tet, or Hexcore volume meshing parameters, as appropriate. Descriptions of meshing parameters

are found in Prism Meshing Options for Scoped Prisms (p. ), Generating Tetrahedral Meshes (p. ),

and Generating the Hexcore Mesh (p. ).

After setting mesh parameters, you can compute the mesh in an individual volumetric region

using the Auto Fill Volume option. See Meshing Regions Selectively Using Auto Fill

Volume (p. ).

b.

To apply meshing parameters and compute the volume mesh collectively for all volumetric regions

of the selected object(s), use the Auto Mesh option in the Volumetric Regions context menu. See

Meshing All Regions Collectively Using Auto Mesh (p. ).

You can also access the Auto Mesh option from the object level context menu, and access

the scoped prism option directly using Setup Scoped Prisms... from the Volumetric Regions

menu.

.

Examine the volume mesh and verify the mesh quality.

a.

The computed volume mesh is placed into Cell Zones.You can use the context menus to draw the

cell zones individually or collectively to examine the mesh. Cell zones may be merged or deleted if

necessary.Volumetric regions are not affected if cell zones are deleted. Refer to Cell Zone Op-

b.

Improve the mesh quality using the Auto Node Move tool, if needed. See Moving Nodes (p. ).

When you are satisfied with the quality of the volume mesh, prepare the mesh for transfer to solution

mode. Right click on Model at the top of the tree and select Prepare for Solve from the context menu.

Operations such as deleting dead zones, deleting geometry objects, deleting edge zones, removing

face/cell zone name prefixes and/or suffixes, and deleting unused faces and nodes are performed during

this operation.

Important

In object-based workflows, merging cell zones requires that they be in the same volumetric

region.

To merge cell zones that cannot be in the same volumetric region because they are not

Important

region.

contiguous, you will need to first delete the object(s) only, and then use the Manage Cell

Zones dialog box.

Note

When you generate a poly mesh, node weights for node-based gradients are enabled by

default. For postprocessing, this setting can improve the accuracy of the displayed results

near wall edges when you are displaying contours on the poly mesh. When you transfer the

poly mesh to solution mode, a message will notify you that this interpolation is enabled.

You can disable it by setting the /display/set/nodewt-based-interp? command

to no.

Volumetric regions are finite, contiguous domains that are ready for volume meshing. Volumetric regions

are computed from the conformal surface mesh and material points. If a volumetric region is changed,

you should validate or update the regions prior to filling with the volume mesh.

You can use the context-sensitive menu available for Volumetric Regions for managing the regions

collectively:

Object-Based Volume Meshing

Use Compute to initialize the regions; Validate to confirm the finite, contiguous domains after changes;

and Update to preserve names and types while recalculating regions.

You can use the Select Regions and External Baffles sub-menus to assist in selecting or visualizing

regions based on type.

Object-based meshing parameters are set and the volumetric regions filled using the Auto Mesh tool.

The Setup Scoped Prisms... tool is a direct link to the Scoped Prisms dialog box.

You can get surface mesh statistics using the Summary option, and a listing of region composition

using the Info option.

Individually, you can use the context-sensitive menu for a named volumetric region to modify and ex-

amine the region, as well as set up regional mesh parameters.

Use Draw, Draw Options, and List Selection to assist in selecting and visualizing the regions.

The tools available in the Diagnostics..., Change Type, Manage, and Remesh Faces menus are

used to modify the volumetric region.

You can set up regional mesh parameters using the Scoped Prisms, Tet, and Hexcore menus.The

Auto Fill Volume... tool is used to generate the volume mesh for the individual region.

Delete Cells will remove any existing volume mesh while preserving the volumetric region information.

You can get surface mesh statistics using the Summary option and the region's composition using the

Info option.

The available options are described in detail in the following sections.

... Computing and Verifying Regions

...Volumetric Region Operations

The controls described here are found in the context-sensitive menu accessed by right-clicking on

Volumetric Regions.

Compute

Volumetric regions need to be computed prior to object based volume meshing.The Compute Regions

dialog box contains options for computing volumetric regions to produce ready to mesh domains.The

computing of regions includes topology checks, re-orienting of normals, and baffle identification and

handling before generating the volume mesh.

The volumetric region computation can also handle overlapping zones, so long as they are not

multi-connected.

.

Select Compute... to open the Compute Regions dialog box.

Volumetric Region Management

.

Select the material points in the Material Points selection list and click OK.

Note

When regions are computed, region names and types will be based on the face zone

labels of the mesh object selected. If regions are recomputed, all previous region names

and types will be over written.

Validate

Volumetric regions must be closed, water-tight domains. If individual regions are modified after initially

computing volumetric regions, the modified regions need to be validated before proceeding to volume

meshing. Regions can be modified using operations such as merging, deleting, or renaming them or

changing the region type. Also, the region may also be modified if scoped prism settings are applied.

To manually validate the volumetric regions, select Validate. Also, the regions will be validated

when the volume mesh is generated.

Update

Some of your modifications may involve changing the name or type for the volumetric region.You can

recalculate the volumetric region without affecting the region name or type using the Update control.

Select Regions

Connects to a sub-menu that allows you to select multiple regions based on type (fluid, solid, dead, or

all).

External Baffles

Connects to a sub-menu that allows you to display, select, or remove the baffle(s) from the volumetric

regions.

Setup Scoped Prisms

Provides direct access to Scoped Prisms dialog box in which you can define inflation layers to specific

regions.

entities in the model.

Auto Mesh

Use this menu item for setting up volume fill meshing parameters and computing the volume mesh in

the full object.

Summary

From the Volumetric Regions menu, you can use Summary to obtain an overall summary with counts

of face zones, all, free, multi, and duplicate faces, the maximum skewness and number of faces with

skewness > ..

Info

From the Volumetric Regions menu, you can use Info to obtain a listing of all regions with type, volume,

material point, and face zones.

The context-sensitive menus for individual volumetric regions offer several options to select or draw

regions. With one or more regions selected in the tree:

Use the Draw menu item to draw the highlighted region(s), replacing what was previously displayed.

Use the Draw Options submenu to add, remove, highlight, or select the region(s) to (from) the display.

This submenu also provides options to draw, add, remove, highlight, or select regions based

on boundary type (Walls or Baffles), interface type (Fluid-Fluid interface, Fluid-Solid interface,

or Solid-Solid interface), or volume type (Filled Volume or Empty Volume).

Use the List Selection submenu to add, remove, or select the region(s) to (from) a selection list in a

This submenu also provides options to select, add, or remove regions based on boundary type

(Walls or Baffles), interface type (Fluid-Fluid interface, Fluid-Solid interface, or Solid-Solid

interface), or volume type (Filled Volume or Empty Volume).

Operations to modify the selected volumetric region(s) include the following:

Face connectivity and quality based diagnostic tools are available for fluid volumetric regions. Select Dia-

gnostics... in the menu available for the region selected to open the Diagnostic Tools dialog box.

Use the Change Type option to change the region type in the corresponding drop down list.

Merge multiple regions using the Manage  → Merge... option in the menu. Enter the New Region Name

and select the type for the merged region in the New Region Type drop-down list in the Merge Regions

Note

If there are shared face zones, merging regions will delete the shared face zones. However,

if there are cell zones associated with the regions, then merging the regions will not delete

the shared face zones. In this case, the shared face zones will be deleted when the cell

zones are deleted.

Rename individual regions using the Manage → Rename option in the menu. Enter the New Region Name

in the Rename Region dialog box.

Delete regions using the Manage → Delete option in the menu.

Tip

Deleting regions may cause face zones to be deleted. It is recommended that the region

type be changed to dead instead of deleting the region.

Use the Remesh Faces option in the menu to remesh the face zones based on the existing size field.

Volume meshing operations include options to set up meshing parameters, fill the volume based on

the parameters set, and manipulate the cell zones in the regions.

Use the Scoped Prisms → Set... option to open the Scoped Prisms dialog box for setting scoped prism

controls.

Use the Tets → Set... option to open the Tet dialog box for setting tetrahedral mesh controls.

controls.

Use the Hexcore → Set... option to open the Hexcore dialog box for setting hexcore mesh controls.

Use the Auto Fill Volume... option to open the Auto Fill Volume dialog box to create the volume mesh

for the selected volumetric regions based on the meshing parameters set.

Use the Delete Cells option to delete the cell zones of the volumetric regions.

The Summary and Info options print information to the console about the surface mesh and the region's

composition, respectively, for the selected volumetric region(s).

When regions have been computed and verified, you can proceed to generate the volume mesh. Use

the process described below that is best suited to your workflow or problem:

... Meshing All Regions Collectively Using Auto Mesh

... Meshing Regions Selectively Using Auto Fill Volume

Note

The workflow for object-based volume meshing does not support partial meshing within a

region. Operations such as prisms generation only, Tet-initialization only, Hexcore only, etc.,

require a domain-based workflow.

Important

In the object-based volume meshing procedure, by default a backup of the surface mesh is

created before volume meshing starts. To restore the surface mesh at any point, select Restore

Faces in the context-sensitive menu for the mesh object. When you select the Restore Faces

option, the current object face zones and cell zones will be deleted.

To disable the backup, set the /mesh/auto-mesh-controls/backup-object command

to no. In that case, you will not be able to restore the surface mesh using the Restore Faces

option.

option.

There may be a difference in the initial volume mesh generated for an object and that gen-

erated after restoring the object surface mesh due to differences in the order of zones/entities

processed during volume meshing.

The Auto Mesh dialog box contains options for generating the volume mesh for all computed volu-

metric regions of the mesh object.

The volume mesh can be generated as follows:

.

Open the Auto Mesh dialog box from the context-sensitive menu available by right-clicking on any

mesh object or its Volumetric Regions or Cell Zones branch in the tree.

You can also use the Mesh → Auto Mesh menu item to open the Auto Mesh dialog box.

.

Ensure that the mesh object is selected in the Object drop-down list.

Note

If you open the Auto Mesh dialog box from the context-sensitive menu in the tree,

the mesh object to which the cell zones, or volumetric regions, belong is automatically

selected.

.

Enable/disable Keep Solid Cell Zones and Keep Dead Cell Zones, as required.

.

Select the appropriate option in the Grow Prisms drop-down list in the Boundary Layer Mesh group

box.

a.

Retain the default selection of none if you do not need to grow prism layers for the current meshing

approach.

b.

Select scoped if you want to specify object-based prism controls. Click Set... to open the Scoped

Prisms dialog box and define the prism controls for the mesh object. Refer to Prism Meshing Options

for Scoped Prisms (p. ) for details.

Tip

Tip

You can save your scoped prism controls to a file (*.pzmcontrol) for use in batch

mode, or read in a previously saved scoped prism file.

c.

Select zone-specific if you want to specify zone-specific prism parameters. Click Set... to open the

Prisms dialog box and specify the zone-specific prism parameters. Refer to Procedure for Creating

Zone-based Prisms (p. ) for details.

Note

Poly meshing does not support zone-specific prisms.

.

Select the appropriate quad-tet transition elements from the Quad Tet Transition list. Click the Set...

button to open the Pyramids dialog box or the Non Conformals dialog box (depending on the selection)

and specify the appropriate parameters. Refer to Creating Pyramids (p. ) and Creating a Non-Conformal

Interface (p. ) for details.

Note

The Quad Tet Transition options are not applicable to poly mesh.

.

Select the appropriate option from the Volume Fill list. Click the Set... button to open the Tet, Hexcore,

or Poly dialog box (depending on the selection). Specify the appropriate parameters. Refer to Initializing

Generating the Volume Mesh

the Tetrahedral Mesh (p. ), Refining the Tetrahedral Mesh (p. ), Controlling Hexcore Parameters (p. ),

and Generating Polyhedral Meshes (p. ) for details.

Note

The No Fill option is not available when a mesh object is selected for volume meshing.

Some operations such as prisms generation only,Tet-initialization only, Hexcore only, are

not available for object-based volume meshing. Similarly, options under the Zones group

in the Tet and Hexcore dialog boxes, that require a zone-based workflow, have no effect

for object-based volume meshing.

.

Specify the appropriate Volume Fill Options.

a.

For the Tet or Poly methods, set the following:

Select the appropriate option for Cell Sizing.

– Size Field specifies that the cell size is determined based on the current size-field.

– Geometric specifies that the cell size in the interior of the domain is obtained by a geometric

growth from the closest boundary according to the growth rate specified.

Set the Growth Rate required.

Specify the Max Cell Length. Click Compute to compute the maximum cell size based on the

b.

For the Hexcore method, set the following:

Select the appropriate option for Type.

Retain the default selection of Cartesian or select the Octree type.

Set the number of Buffer Layers and Peel Layers.

Specify the Max Cell Length for the Cartesian approach. Click Compute to compute the maximum

cell size based on the mesh object.

Specify the Min Cell Length for the Octree approach.

.

Enable or disable additional Options as desired.

Enable Merge Cell Zones within Regions to create a single cell zone within a region, or disable to

keep the cell zones separate.

.

Click Mesh in the Auto Mesh dialog box.

Alternatively, you can use the command /mesh/auto-mesh to generate the mesh automatically.

Specify a mesh object name for object-based auto mesh; if no name is given, face zone based auto

mesh is performed. Specify the mesh elements to be used when prompted. Specify whether to merge

the cells into a single zone or keep the cell zones separate. For face zone based meshing, specify

whether to automatically identify the domain to be meshed based on the topology information.

Note

You can specify the meshing parameters for the mesh elements (prisms, pyramids or

non-conformals, tet, or hex) using either the respective dialog boxes or the associated

text commands prior to using the auto-mesh command. Commands for poly meshes

are located under the mesh/poly menu.

The Auto Fill Volume dialog box contains options for generating the volume mesh in selected volu-

metric regions for mesh objects.

.

In the tree, expand Volumetric Regions and select the regions to be meshed.

.

Set up the regional meshing parameters for the selected regions.

a.

Specify scoped prism controls for the boundary layer mesh, if applicable. Select Scoped Prisms →

Set... in the context-sensitive menu to open the Scoped Prisms dialog box. Refer to Prism Meshing

Options for Scoped Prisms (p. ) for details.

b.

Specify tetrahedral mesh or hexcore mesh parameters, as applicable.

Select Tets → Set... to open the Tet dialog box. Refer to Initializing the Tetrahedral

Mesh (p. ), and Refining the Tetrahedral Mesh (p. ) for details.

Select Hexcore → Set... to open the Hexcore dialog box. Refer to Controlling Hexcore Para-

meters (p. ) for details.

Note

When you click the Compute button in the Tet or Hexcore dialog box, you will

be asked if the maximum cell size is to be computed based on the mesh object

selected. Click Yes to recompute the cell sizes based on the mesh object.

Alternatively, open the Auto Fill Volume dialog box from the menu for the selected regions. Click

the Set... button in the Boundary Layer Mesh and Volume Fill group box to set the scoped

prism and tetrahedral/hexcore mesh parameters, respectively.

.

Set the boundary layer mesh and volume fill options in the Auto Fill Volume dialog box.

a.

Enable Grow Scoped Prisms if scoped prism controls have been set up.

b.

Select Tet or Hexcore in the Volume Fill list.

.

Click Mesh in the Auto Fill Volume dialog box.

Repeat this procedure for any empty volumetric regions until all regions are filled.

The context-sensitive menu for Cell Zones contains options for visualizing and manipulating all cell

zones collectively:

Use Draw All Boundaries to draw all the cell zone boundaries or Draw All Cells in Range to draw

all the cells within a specified range (for either unreferenced or referenced zones). The range can be

set in the Bounds group in the ribbon.

Use Auto Mesh... to access the Auto Mesh tool for volume meshing.

Use Auto Node Move... to access the Auto Node Move tool for improving the mesh quality by moving

nodes.

Use the Select Cell Zones sub-menu for selection of all cell zones as well as selection by type (fluid, solid,

or dead).

Use Delete All to delete all cell zones, if needed.

Use Summary to obtain an overall summary of cell count and quality or Info to obtain individual cell zone

type and cell zone count by type.

The context-sensitive menu for individual cell zones offers several options to select or draw cell zones.

Use Draw Boundaries to draw the boundaries of the selected zones, or Draw Cells in Range to draw the

cells within a specified range.

Use the Draw Options submenu to add, remove, highlight, or select the cell zone(s) to (from) the display.

Use the List Selection submenu to add, remove, or select the cell zone(s) to (from) a selection list in a dialog

box.

Use Auto Node Move... to access the Auto Node Move tool for improving the mesh quality of the selected

zone by moving nodes.

Use Merge to combine two or more selected cell zones into a single zone.

Important

region.

Use Delete to delete the cell zones, if needed.Volumetric regions are not affected if cell zones are deleted.

Use Summary to obtain a summary of cell count and quality or Info to obtain individual cell zone type and

cell zone count by type.

Chapter : Manipulating the Boundary Mesh

The first step in producing an unstructured mesh is to define the shape of the domain boundaries. You

can create a boundary mesh in which the boundaries are defined by triangular or quadrilateral facets

using a preprocessor (GAMBIT or a third-party CAD package) and then create a mesh in the meshing

mode in Fluent. You can also modify the boundary mesh to improve its quality and create surface

meshes on certain primitive shapes. The following sections discuss mesh quality requirements and

various techniques for generating an adequate boundary mesh for numerical analysis.

.. Manipulating Boundary Nodes

.. Intersecting Boundary Zones

.. Modifying the Boundary Mesh

.. Improving Boundary Surfaces

.. Refining the Boundary Mesh

.. Creating and Modifying Features

.. Remeshing Boundary Zones

.. Faceted Stitching of Boundary Zones

..Triangulating Boundary Zones

.. Separating Boundary Zones

.. Projecting Boundary Zones

.. Creating Groups

.. Manipulating Boundary Zones

.. Manipulating Boundary Conditions

.. Creating Surfaces

.. Removing Gaps Between Boundary Zones

.. Using the Loop Selection Tool

Manipulation of boundary nodes is an effective way to influence the boundary mesh quality. Operations

for deleting unwanted boundary nodes can be performed in the Merge Boundary Nodes dialog box

or with the associated text commands.

... Free and Isolated Nodes

The mesh generation algorithm does not permit duplicate nodes; that is, two nodes that have the

same Cartesian coordinates. Duplicate nodes may be created by mesh generators that preserve the

node locations at adjoining edges of adjacent surfaces, but give different labels to the two sets of

nodes. The nodes and edges at which these surfaces meet are termed free nodes and free edges.

Figure . : Free Nodes

Figure . : Free Nodes (p. ) shows a simple geometry in which the free nodes are marked. Although

the node at the end of curve C1 (N12) is located in the same position as the node at the beginning

of curve C2 (N21), each is a free node because it is not connected in any way to the adjoining curve.

Though the nodes have the same location, the mesher knows only that they have different names,

and not that the curves meet at this location. Similarly, a free edge is a surface edge that is used by

only one boundary face. To check the location of free nodes, use the Display Grid dialog box. Free

edges are acceptable when modeling a zero-thickness wall (“thin wall") in the geometry (for example,

Figure . : Example of a Thin Wall (p. )). Isolated nodes are nodes that are not used by any

boundary faces. You can either retain these nodes to influence the generation of the interior mesh

(see Inserting Isolated Nodes into a Tet Mesh (p. )), or delete them.

Figure . : Example of a Thin Wall

You can connect triangular boundary zones in the geometry using the set of intersection operations

available. These can be used to resolve intersections, overlaps, and for connecting zones along the free

boundaries.

... Intersecting Zones

... Joining Zones

Manipulating the Boundary Mesh

... Stitching Zones

... Using the Intersect Boundary Zones Dialog Box

... Using Shortcut Keys/Icons

The intersect option is used to connect intersecting tri boundary zones. Figure . : Intersection of

Boundary Zones (p. ) shows an example where the intersect option can be used. The connection is

made along the curve (or line) of intersection of the boundary zones. You can use the intersection

operation on multi-connected faces as well as in regions of mesh size discrepancy.

Figure . : Intersection of Boundary Zones

To intersect boundary zones with a gap between them, specify an appropriate Tolerance value. All

zones with the distance between them less the specified tolerance value will be intersected. The toler-

ance can be either relative or absolute. When intersecting zones having different mesh sizes, you can

use the Refine option to obtain a better graded mesh around the intersecting faces (see Figure . : In-

tersection (A) Without and (B) With the Refine Option (p. )).

Figure . : Intersection (A) Without and (B) With the Refine Option

Intersecting Boundary Zones

The join option is used to connect two overlapping tri boundary zones (Figure . : Partially Overlapping

Faces (p. )). The overlapping areas of both the boundary zones are merged and the mesh at the

boundary of the region of overlap is made conformal. To join surfaces that are on top of each other

but not connected (with a small gap), specify an appropriate Tolerance value. The portion of the surfaces

within the tolerance value will be joined. The boundary zone selected in the Intersect Tri Zone defines

the shape of the combined surface in the overlap region. The shape in the With Tri Zone may be

changed to perform the join operation.

Figure . : Partially Overlapping Faces

Figure . : Joining of Overlapping Faces (p. ) and Figure . : Remeshing of Joined Faces (p. )

show the overlapped faces after joining and after remeshing the joined faces.

Figure . : Joining of Overlapping Faces

Figure . : Remeshing of Joined Faces

Tip

In case of completely overlapping face zones, you may need to separate the zones and then

join individual pairs. In such cases, you may use the /boundary/check-duplicate-

geom command to delete the duplicate face zone instead.

The stitch option is used to connect two tri boundary zones along their free edges. You cannot use

this option to connect the surfaces at a location other than the free edges in the mesh. Gaps within

the given tolerance are closed using nearest point projection.

Figure . : Nearest Point Projection for Stitching

Figure . : Nearest Point Projection for Stitching (p. ) shows a cut through the two surfaces, Face-

and Face-, that are separated by a gap. The points of nearest projection will determine the location

of the intersection curve. Therefore, point- will be connected to point- or point-. All three

connect operations allow a small gap (within the tolerance specified) between the intersecting

boundary zones; however, the gap should not distort the shape of the geometry.

Figure . : Surfaces Before Stitch (p. ) and Figure . : Surfaces After Stitch (p. ) show the surfaces

before and after the stitch operation, respectively

Figure . : Surfaces Before Stitch

Figure . : Surfaces After Stitch

In general, all three connect operations calculate the intersection curve (or line) between the two

surfaces to be connected. The intersection curve is constructed as follows:

Intersect constructs the curve as the intersection of two zones.

Join constructs the curve as the outer boundary of the overlapping region within the specified tolerance

of the two surfaces.

Stitch constructs the curve along the free boundaries and within the specified tolerance.

The intersection curve is remeshed with a local spacing calculated from the intersecting surfaces. The

intersection curve is inserted into the surfaces and will result in a retriangulation of the surfaces along

the intersection curve.

The /boundary/remesh/remesh-overlapping-zones command extracts the boundary edge

zones from the zone to imprint. The intersecting curve is inserted into the zones. During the insertion,

the zones are retriangulated.

After any connect operation, remesh is called automatically. To disable the post-remesh operation, use

the text command:

/boundary/remesh/controls/intersect/remesh-post-intersection? no

To perform any of the intersection operations, do the following:

.

Select the boundary zones you want to intersect in the Intersect Tri Zone list.

.

Select the boundary zones with which you want to intersect the selected boundary zone in the With Tri

Zone list.

.

Select the appropriate operation from the Operation list.

.

Specify the appropriate Tolerance value (if the surfaces have a gap between them).

.

Enable Absolute Tolerance, Refine, or Separate as appropriate.

.

Click Mark.

.

.

.

The faces that will be affected by the intersection operation are highlighted. This also helps you

decide whether the specified tolerance is appropriate.

.

You can use the Join dialog box to join overlapping face zones based on selections in the graphics

window.

. Alternatively, use the hot-

key Ctrl+T to invoke the miscellaneous tools and then Ctrl+J to open the Join dialog box.

The detailed procedure is described in Using the Join Dialog Box (p. ).

You can use the Intersect dialog box to join overlapping face zones based on selections in the

key Ctrl+T to invoke the miscellaneous tools and then Ctrl+I to open the Intersect dialog box.

The detailed procedure is described in Using the Intersect Dialog Box (p. ).

Tools are available for making boundary repairs, enabling you to perform primitive operations on the

boundary mesh, such as creating and deleting nodes and faces, moving nodes, swapping edges, merging

and smoothing nodes, collapsing nodes, edges, and faces, splitting faces, and moving faces to another

boundary zone.

... Using the Modify Boundary Dialog Box

... Operations Performed: Modify Boundary Dialog Box

... Locally Remeshing a Boundary Zone or Faces

... Moving Nodes

This section describes the generic procedure for modifying the boundary mesh using the Modify

Boundary dialog box. In addition to the Modify Boundary dialog box, you may also use the Display

Grid dialog box during the modification process.

.

Display the boundary zones that you want to modify, using the Display Grid dialog box. If you need to

modify many zones, display them one at a time to make the graphics display less cluttered.

.

Select the type of entity you want to select with the mouse: edge, node, position, and so on in the Filter

list in the Modify Boundary dialog box.

.

Select the entities you want to operate on using the mouse-probe button (a right-click, by default) in

You can select individual entities one at a time, or select a group of them by defining a selection

region. See Controlling the Mouse Probe Function (p. ) for details. The selected entities will

appear in the Selections list in the Modify Boundary dialog box.

.

Click the appropriate Operation button to perform the boundary modification.

The mesh is automatically re-displayed after the operation is performed, enabling you to immedi-

ately see the effect of your change.

.

Repeat the process to perform different operations on different entities.

Warning

Save the mesh periodically as it is not always possible to undo an operation.

You can perform the following operations using the Modify Boundary dialog box:

Creating Nodes

To create nodes, do the following:

.

.

Select the required positions (or enter node coordinates explicitly in the Enter Selection box).

.

Select node in the Filter list or press Ctrl+N.

.

Click Create or press F5.

Creating Faces

To create a face, do the following:

.

Select  or  nodes and the optional zone.

Use the hot keys Ctrl+N and Ctrl+F to select node and face as Filter, respectively.

.

While creating a face:

If you do not select a zone, the new face will be in the same zone as an existing face that uses one of the

specified nodes.

If the nodes you use to create a face are used by faces in different zones, make sure that the new face is in

the right zone.

Modifying the Boundary Mesh

If you create a face and it is in the wrong zone, use the rezoning feature.

Creating a Zone

To create a new zone, do the following:

.

Select zone in the Filter list (or Ctrl+Z).

.

Click Create or press F5.The Create Boundary Zone dialog box will open, prompting you for the zone

name and type.

.

Specify the name and zone type as appropriate in the Create Boundary Zone dialog box.

.

Click OK.The new zone will automatically be added to the Selections list in the Modify Boundary dialog

box.

Deleting a Node/Face/Zone

To delete the nodes or faces, do the following:

.

Select the nodes or faces or zones to be deleted.

.

Click Delete or press Ctrl+W on the keyboard.

Merging Nodes

To merge nodes, do the following:

.

Select the two nodes to be merged.

.

Click Merge or press F9.

Important

The first node selected is retained; the second node is merged onto the first node.

Tip

.

.

Important

Tip

You can merge multiple pairs of nodes by selecting an even number of nodes, in the correct

order, before clicking Merge (or pressing F9). The first and second nodes will be merged,

then the third and fourth, and so on.

Moving Nodes

To move the node to any position in the domain, do the following:

.

Select node in the filter list (or Ctrl+N).

.

Select the node you want to move.

.

Choose position in the filter list (or Ctrl+X).

.

Select the position coordinates or click the position in the graphics window to which you want to move

the selected node.

.

Click Move To.

To move the node by specifying the magnitude of the movement, do the following:

.

.

.

Enter the magnitude by which you want to move the selected node.

.

Click Move By.

Rezoning Faces

To rezone one or more faces, do the following:

.

Select the faces you want to move.

.

Select the zone to which you want the selected faces to move.

.

Click Rezone (or Ctrl+O).You can create a zone if you need to move faces to a new zone.

Collapsing Nodes/Edges/Faces

To collapse nodes, edges, or faces, do the following:

.

Select the appropriate Filter.

.

Select the two nodes (or edges/faces) you want to collapse.

.

Click Collapse (or Ctrl+^).

While collapsing:

If a pair of nodes is selected, both the nodes are moved towards each other (at the midpoint) and collapsed

into a single node.

If an edge is selected, the two nodes of the edge collapse onto the midpoint of the edge and surrounding

nodes are connected to the newly created node.

If a triangular face is selected, a new node is created at the centroid of the triangle and the selected trian-

gular face gets deleted.

Note

You can also collapse multiple pairs of entities by selecting multiple entities before clicking

Collapse. Ensure that an even number of entities is selected. The first and the second entity

will be collapsed, then the third and the fourth, and so on.

Smoothing Nodes

To smooth nodes, do the following:

.

Select the nodes you want to smooth.

.

Click Smooth or press F6.

The node will be placed at a position computed from the average of the surrounding nodes.

Splitting Edges

To split edges, do the following:

.

Select the edges you want to split.

.

Click Split or press F7.

All faces sharing the edge will be split into two faces.

If you select multiple edges and they share a face, the split operation may not be completed. If the

face referenced by the split operation for the second edge has already been split by the operation on

the first edge, the second split operation will not be possible because the referenced face that no

longer exists. If this happens, redisplay the mesh and reselect the edge that was not split. In such cases

it may also be easier to split the face rather than the edge.

Splitting Faces

To split faces, do the following:

.

Select the faces you want to split.

.

Each triangular face will be split into three faces by adding a node at the centroid. Each quadrilat-

eral face will be split into two triangular faces.

.

Perform edge swapping after this step to improve the quality of the local refinement.

Swapping Edges

To swap an edge of a triangular face, do the following:

.

Select the edges as appropriate.

.

Click Swap or press F8. If the triangular boundary face on which you perform edge swapping is the cap

face of a prism layer, the swapping will automatically propagate through the prism layers, as described

in Edge Swapping and Smoothing (p. ).

Note

Edge swapping is not available for quadrilateral faces.

Finding Coordinates of the Centroid

To find the location of the centroid of a face or cell, do the following:

.

Set Filter to face or cell as appropriate.

.

Select the face or the cell using the mouse probe button.

.

Click the Centroid button (or Ctrl+L).

The face or cell centroid location will be printed in the console window.

Calculating Distance Between Entities

To compute the distance between two entities, do the following:

.

Set Filter to face, edge, or cell as appropriate.

.

Select the two entities.

.

Click Distance (or Ctrl+D).

For example, if an edge (or face or cell) and a node are selected, the distance between the centroid

of the edge (or face or cell) and the node is computed and printed to the console window.

Projecting Nodes

To reconstruct features in the surface mesh that were not captured in the surface mesh generation,

project selected nodes onto a specified line or plane.

The Create Boundary Zone dialog box will appear automatically when you create a new face zone.

You can specify the name and type of the new zone in this dialog box.

To project nodes, do the following:

.

Define the projection line or plane. For a projection line, select two entities and for a projection plane,

select three entities. If edges, faces, or cells are selected, their centroidal locations will be used.

.

Click Set (or Ctrl+S) and the projection line or plane will be shown in the graphics display.

.

Select the nodes to be projected.

.

Click Project (or Ctrl+P).

The selected nodes are projected onto the projection line or plane that you defined with the Set

operation.

Simplifying Boundary Modification

The following functions simplify the boundary modification process:

Finding the Worst/Marked Faces

You can display faces in the descending order of their quality as follows:

.

To find the face having the worst quality in the mesh, select Quality Limit and click First or press F11.

The worst face will be displayed in the graphics window and its quality and zone ID are reported

in the console.

The longest edge of the face and the node opposite it are selected, and the display is limited to the

neighborhood of the highly skewed face.

If the mesh has not been displayed, the worst face, its quality, and the zone in which it lies will be re-

ported (in the console).

.

Click Next (or the right-arrow key).

The face having the next higher quality will be displayed in the graphics window. When you

subsequently click Next, the face having the next higher quality (after that of the previously dis-

played or reported face) will be displayed or reported.

.

.

Click Reset (or the left-arrow key) to reset the display to the worst quality element.

You can also find the worst face within a subset of zones by activating a group containing the required

zones using the User Defined Groups dialog box and then clicking First. When you click the Next

button after activating a particular group, the face having the next higher quality within the active

group will be displayed. (Ensure that the global group is activated to have all the zones available.)

To display the marked faces in succession, do the following:

.

Select Mark and click First (or F11) to find the first marked face.

The face will be displayed in the graphics window.

.

The next marked face is displayed in the graphics window.

.

Click Reset (or the left-arrow key) to reset the display to the first marked face.

You can use the /bounday/unmark-selected-faces command (or Ctrl+U) to unmark the

faces.

To improve the quality of the face, use the following operations:

Use the Smooth operation to smooth the node opposite the longest face.

Use the Merge operation to collapse the shortest edge of the face, merging the other two edges together.

The longer of the remaining two edges is retained, while the shorter one is merged with the other edge.

Use the Swap operation to swap the selected edge.

Use the Split operation to refine the face by bisecting the selected edge.

If the selected entities are not appropriate, clear them, choose the appropriate items, and perform the

desired operations.

Deselecting a Selected Entity

If you select an inappropriate entity, you can click on it again in the graphics window to deselect it.

You can also select it in the Selections list in the Modify Boundary dialog box and click Clear. You

can use F2 to deselect all entities selected.

Warning

Deselect operations are performed only on the items selected in the Selections list.

Undoing an Operation

To undo an operation, click Undo or press F12. In some cases, a particular sequence of operations

cannot be undone. Hence, make sure that you save the mesh periodically between the modifications.

Click Undo or press F12 n times to undo the last n operations.

Warning

The Undo operation is limited to the operations in the Modify Boundary dialog box (or

the /boundary/modify menu). If other operations/commands are interleaved, the Undo

operation may cause unexpected results.

Note

You can also fix holes in the geometry. Refer to Fixing Holes in Objects (p. ) for details.

The Zone Remesh dialog box contains options for remeshing face zones selected in the graphics

window. To remesh face zones, select them in the graphics window and press Ctrl+Shift+R to open

the Zone Remesh dialog box.

.

Select the sizing source (size-field or constant-size).

.

Specify the feature angle to be preserved while remeshing the selected zones.

.

Specify the Constant Size value when the constant-size method is selected.

The Preview button allows you to display size boxes to visualize the proposed constant size.

.

.

.

The Local Remesh dialog box contains options for remeshing marked faces or faces based on selections

in the graphics window. Select the faces in the graphics window. Press Ctrl+Shift+J for face marking

options. After selecting/marking the faces, press Ctrl+Shift+R to open the Local Remesh dialog box.

.

Set the number of radial layers of faces to be remeshed in the Rings field.

.

Specify the feature angle to be preserved while remeshing the selected faces.

.

Select the sizing source (geometric, size-field, or constant-size).

.

.

To specify a distance and direction for moving a node using the Move Nodes dialog box, do the fol-

lowing:

.

Select a Seed Node from your model.

.

Set the number of nodes to move in the Node Count box.

.

Set the move distance in the Move by box.

.

Select a direction.

Seed-Normal moves all the nodes in parallel to the seed node normal.

Local-Normal moves each node in the direction of its own normal.

Flip moves the nodes in the opposite direction.

.

Use Draw to preview the direction and distance selected.

You may use the Boundary Zones selection list and Boundary Zone Groups list along with Draw to

isolate the zone of interest in the display.

The quality of the volume mesh is dependent on the quality of the boundary mesh from which it is

generated. You can improve boundary surfaces to improve the overall mesh quality.

You can improve the boundary mesh by specifying an appropriate quality limit depending on the

quality measure considered. You can also smooth and swap faces on the boundary surfaces to improve

the mesh quality. You can use the Boundary Improve dialog box to improve the surfaces. You can

diagnostically determine the boundary mesh quality using the Check and Skew buttons available when

the Swap option is selected.

... Improving the Boundary Surface Quality

... Smoothing the Boundary Surface

... Swapping Face Edges

You can improve the boundary surface quality using skewness, size change, aspect ratio, or area as

the quality measure.

For improving the boundary surface quality based on skewness, size change, and aspect ratio, specify the

quality limit, the angle, and the number of improvement iterations. All the elements above the specified

quality limit will be improved.

For improving based on the area, collapse faces and then either swap the edges or smooth the surface. All

faces having area smaller than the specified minimum absolute size will be collapsed.

You can also specify the minimum relative size (size of the neighboring entity) to be considered while

using the Collapse and Swap option.

Smoothing of the surface mesh allows you to control the variation in the size of the mesh elements,

thereby improving the accuracy of the numerical analysis. Smoothing is critical in regions of proximity

or regions where surfaces intersect and the accuracy of the approximations used in numerical analysis

techniques deteriorates with rapid fluctuations in the element size. The smoothing procedure involves

relocating of the mesh nodes without changing the mesh topology.

Edge swapping can be used to improve the triangular surface mesh. The procedure involves checking

each pair of faces that shares an edge and identifying the connecting diagonal that results in the most

appropriate configuration of faces within the resulting quadrilateral. For a face considered, if the un-

shared node on the other face lies within its minimal sphere, the configuration is considered to be a

Delaunay violation and the edge is swapped. The procedure makes a single pass through the faces to

avoid cyclic swapping of the same set of edges. Thus, the edge swapping process is repeated until no

further improvement is possible. At this stage, even if a few Delaunay violations exist, the differences

resulting from continual swapping are marginal.

Important

If the triangular boundary zone selected is the cap face zone of a prism layer, the edge

swapping will automatically propagate though the prism layers.

To use refinement regions for local refinement in some portion of the domain (for example, to obtain

a high mesh resolution in the wake of an automobile), you may refine the associated boundary zones

as well. When you perform the local refinement, the boundary faces that border the refinement region

will not be refined. It is therefore possible that you will have a jump in face size where a small cell

touches a large boundary face. To improve the smoothness of the mesh, use the Refine Boundary

Zones dialog box to appropriately refine the boundary zones that border the refinement region before

performing the refinement of the volume mesh. Boundary refinement can be performed only on trian-

gular boundary zones.

... Procedure for Refining Boundary Zones

To refine boundary zones based on marked faces, do the following:

.

Open the Refine Boundary Zones dialog box.

Boundary → Mesh → Refine...

Refining the Boundary Mesh

.

Select Mark in the Options list and define the refinement region. Click the Local Regions... button to

open the Boundary Refinement Region dialog box. Define the refinement region as appropriate.

.

Select the zones to be refined in the Tri Boundary Zones list.

.

Select the region to be refined in the Regions list.The Max Face Area will be updated based on the

value specified in the Boundary Refinement Region dialog box.

.

Click Apply to mark the faces to be refined.

The faces in the selected zones having face area greater than the Max Face Area specified will

be marked.

.

Select Refine in the Options list and Mark in the Refinement group box.

.

The marked faces are refined by dividing them into three faces:

Figure . : Refining a Triangular Boundary Face

To refine boundary zones based on proximity, do the following:

.

.

.

Select Refine in the Options list and Proximity in the Refinement group box.

.

Select the zone from which the proximity is to be determined in the Tri Boundary Zones selection list.

.

Specify the Relative Distance and number of refinement iterations as appropriate.

.

The faces in the proximity of the specified zone are refined as shown here:

Figure . : Boundary Mesh (A) Before and (B) After Refining Based on Proximity

To further improve the quality of the refined boundary mesh, do the following:

.

Select Swap in the Options list and specify the Max Angle and Max Skew as appropriate (use the Refine

Boundary Zones dialog box). See Swapping (p. ) for details about swapping.

.

.

If the geometry of the boundary is close to planar, you can improve the mesh quality further by selecting

the Smooth option, specifying the Max Angle1 and Relax2 parameters, as appropriate (in the Refine

Boundary Zones dialog box), and clicking Apply.

Warning

If the geometry is far from planar, smoothing is not recommended as it may modify

the shape of the boundary.

If you want to repeat the process for another refinement region, first select the Clear option and click

Apply to clear all marks.

Boundary → Mesh → Feature...

Geometric features, such as ridges, curves, or corners should be preserved while performing various

operations (for example, smoothing, remeshing) on the boundary mesh. You can create edge zones for

a face zone and if required, you can also modify the node distribution on the edge zone. The Feature

Modify dialog box contains options available for creating and modifying edge zones. You can also draw

the edge zones to determine their direction (that is, determine the start and the end points).

1Max Angle specifies the maximum angle between two adjacent face normals.When the Swap option is active, only faces with an angle

below this value will be swapped.This restriction prevents the loss of sharp edges in the geometry.The valid range of entries is  to °

and the default is °.The larger the angle, the greater the chance that a face swap will occur that may have an impact on the flow

solution.

2Relax specifies the relaxation factor by which the computed change in node position should by multiplied before the node is moved.

A value of zero results in no node movement, and a value of  results in movement equivalent to the entire computed increment.

Creating and Modifying Features

... Creating Edge Zones

... Modifying Edge Zones

... Using the Feature Modify Dialog Box

Important

For object-based meshing, you can use the context menus in the tree or onscreen tools to create

edge zones on selected face zones or surfaces.These options use the Fixed angle criterion. See

Extract Edge Zones (p. ).

You can also use the Surface Retriangulation dialog box for creating edge zones before

remeshing the face zones.The Surface Retriangulation dialog box allows you to use the face-

zone approach only.

Edge zones can be created according to the specified combination of the edge zone creation approach

and the angle criterion.

The angle criteria used for creating edge zones are as follows:

Fixed angle criterion

This method considers the feature angle between adjacent faces when creating edge zones. You

can specify the minimum feature angle between adjacent faces as a parameter for edge zone creation.

The common edge thread between two faces will be created when the feature angle is greater than

the value specified.

Adaptive angle criterion

This method compares the angle at the edge with the angle at neighboring edges. If the relation

between the angles matches the typical patterns of the angles in the neighborhood of the feature

edge, the edge in question is considered to be a feature edge. You do not need to specify a value

for the feature angle in this case.

The approaches available for edge zone creation are as follows:

Face zone approach

The edge thread is created on the entire face zone based on the specified angle criteria. The face

zone approach is useful when creating edge threads on common edges where two surfaces of the

zone intersect each other. The common edge is considered to be a feature edge when the angle

value specified (fixed angle criterion) is less than the feature angle. Alternatively, the edge thread

at the common edge can be created by detecting the change in the feature angle automatically

(adaptive angle criterion).

Face seed approach

The edge thread is created surrounding the surface on which the seed face is defined based on the

specified angle criteria. The common edge is considered to be a feature edge when the angle value

specified (fixed angle criterion) is less than the feature angle. Alternatively, the edge thread at the

common edge can be created by detecting the change in the feature angle automatically (adaptive

angle criterion).

The Face Seed approach is available only when you use the Feature Modify dialog box for creating

edge zones. If you use the Surface Retriangulation dialog box instead, the Face Zone approach is

used for creating the edge zones.

Figure . : Surface Mesh - Feature Angle =

Figure . : Surface Mesh - Feature Angle =  (p. ) shows a surface mesh with two faces connected

at a common edge and having a feature angle of  degrees. Both faces are in the same face zone.

Figure . : Edge Zone for Face Zone Approach and Fixed Angle =  (p. ) and Figure . : Edge

Zones for Face Seed Approach and Fixed Angle =  (or Adaptive Angle) (p. ) show the edge zones

created for different combinations of approach and angle criterion.

Figure . : Edge Zone for Face Zone Approach and Fixed Angle =  (p. ) shows the single edge zone

created by using the Face Zone approach and Fixed angle criterion, with the angle specified as  degrees.

The edge thread at the common edge is not created as the specified value for Angle is greater than the

feature angle.

Figure . : Edge Zone for Face Zone Approach and Fixed Angle =

Figure . : Edge Zones for Face Zone Approach and Fixed Angle =  (or Adaptive Angle) (p. ) shows

the edge zones created by using the Face Zone approach and Fixed angle criterion, with the angle specified

as  degrees.The interior edge thread at the common edge is created because the specified value for

Angle is smaller than the feature angle. Alternatively, if you use the Adaptive angle criterion, the change

in angle will be detected automatically and the interior edge thread will be created as shown in Fig-

ure . : Edge Zones for Face Zone Approach and Fixed Angle =  (or Adaptive Angle) (p. ).

Figure . : Edge Zones for Face Zone Approach and Fixed Angle =  (or Adaptive Angle)

Figure . : Edge Zone for Face Seed Approach and Fixed Angle =  (p. ) shows the single edge zone

created by using the Face Seed approach and Fixed angle criterion, with the angle specified as  degrees.

The edge thread at the common edge is not created because the specified value for Angle is greater than

the feature angle.

Figure . : Edge Zone for Face Seed Approach and Fixed Angle =

Figure . : Edge Zones for Face Seed Approach and Fixed Angle =  (or Adaptive Angle) (p. ) shows

the edge zones created by using the Face Seed approach and Fixed angle criterion, with the angle specified

as  degrees.The boundary edge thread is created based on the seed face selected.The interior edge

thread at the common edge is created because the specified value for Angle is smaller than the feature

angle. Alternatively, if you use the Adaptive angle criterion, the change in angle will be detected automat-

ically and the boundary and interior edge threads will be created as shown here:

Figure . : Edge Zones for Face Seed Approach and Fixed Angle =  (or Adaptive Angle)

The following edge modification options are available:

Deleting edge zones.

Copying existing edge zones (including the nodes) to a new edge zone.

Toggling the edge zone type between boundary and interior.

Grouping and ungrouping edge zones.

Orienting the edges on the edge zone to point in the same direction.

Reversing the direction of the edge zone.

Note

The direction of a boundary edge zone determines the side from which new faces are

formed. The direction of a boundary edge zone should be right-handed with respect to

the average normal of the face zone to be remeshed. However, the direction is not so

important in the case of interior edge zones because faces are always formed on both

sides of the zone.

Separating the edge zone based on the connectivity and feature angle specified.

Merging multiple edge zones into a single zone.

Note

Only edge zones of the same type (boundary or interior) can be merged.

Remeshing the edge zones to modify the node distribution.

Projecting the edges of the edge zone onto a face zone.

You can select the closest point method or specify the direction in which the edge should be pro-

jected onto the selected face zone.

Intersecting edge zones to create a new edge zone comprising the common edges.

The Feature Modify dialog box can be used for creating edge zones as follows:

.

Select the required zones from the Boundary Zones selection list.

.

Select Create from the Options list.

.

Select the appropriate option from the Approach drop-down list. Select the appropriate Seed Face

when using the Face Seed approach.

.

.

.

.

Select the appropriate option from the Angle Criterion drop-down list. Specify an appropriate value for

the Angle when using the Fixed angle criterion.

.

Enable Add Edges to Object to add the extracted edges to the object comprising the boundary face

zones selected.

.

Click Apply to create the edge zones.

Important

The Feature Modify dialog box can be used for modifying edge loops as follows:

Operations such as deleting, copying, grouping/ungrouping, orienting, separating, and merging edge

loops, toggling the edge loop type, and reversing the edge loop direction:

.

Select the appropriate zones in the Edge Zones selection list.

Warning

You can select only one edge zone when separating an edge zone.

.

Click the appropriate button in the Edge Modify group box.

Remeshing edge zones:

.

Select Remesh from the Options list.

.

Select the appropriate zones from the Edge Zones selection list.

.

Select an appropriate method from the Method drop-down list.You can specify a constant spacing

of nodes or select either the arithmetic or the geometric method for node spacing.You can also select

the Size Field option to use the size field to remesh the edge zones.

For the Constant, Arithmetic, or Geometric methods, set the following parameters:

a.

Specify values for First Spacing and Last Spacing as required.

Note

For the Constant method, the value specified for First Spacing will be the

constant node spacing. Also, the Last Spacing option is not relevant for the

Constant method and will not be available.

b.

Specify an appropriate value for Feature Angle.

c.

Enable Quadratic Reconstruct, if required.The quadratic reconstruction option allows you to

reconstruct the edge by fitting a quadratic polynomial between the original edge nodes.

Alternatively, for remeshing using the size field, make sure the size field is defined as required

(see Computing the Size Field (p. )).

.

Click Apply to remesh the edge zone.

Projecting edge zones:

.

Select Project from the Options list.

.

.

Select the appropriate face zone from the Face Zones selection list.

.

Select the appropriate projection method from the Method drop-down list.The Closest Point

method specifies that the edge should be projected to the closest point on the face zone selected.

The Specific Direction method allows you to project the edge on the face zone in a specific direction.

.

Specify the direction in which the edges should be projected when using the Specific Direction

method.

.

Click Apply to project the edge onto the selected face zone.

Intersecting edge zones:

.

method.

.

.

Select Intersect from the Options list.

.

.

Enable Delete in the Overlapped Edges group box if you want to automatically delete all the over-

lapping edges.

You can use the delete-overlapped-edges text command to delete individual overlapping

edges.

.

Specify an appropriate value for Intersection Tolerance.

.

Click Apply to intersect the selected edge zones.

Boundary → Mesh → Remesh...

In some cases, you may need to regenerate the boundary mesh on a particular boundary face zone.

You may find that the mesh resolution on the boundary is not high enough, or that you want to gen-

erate triangular faces on a boundary that currently has quadrilateral faces. Remeshing of boundary faces

can be accomplished using the Surface Retriangulation dialog box.

You can remesh the boundary face zones based on edge angle, curvature, and proximity.

... Remeshing Boundary Face Zones

... Using the Surface Retriangulation Dialog Box

To remesh a face zone, you first need to create edge zones on the borders of the face zones using the

parameters available in the Edge Create group box in the Surface Retriangulation dialog box (see

Using the Surface Retriangulation Dialog Box (p. )).

You can create the edge zones according to your requirement by specifying an appropriate combination

of the edge zone creation approach and angle criteria (refer to Creating Edge Zones (p. ) for details).

Important

The Face Seed approach is available only when you use the Feature Modify dialog box

for creating edge zones. Click the Feature Modify... button to open the Feature Modify

Note

For object-based meshing, you can create edge zones on selected face zones or surfaces using

the context menus in the tree or onscreen tools.These options use the Fixed angle criterion.

See Extract Edge Zones (p. ).

You can also use the Feature Modify dialog box to create new or modify existing edge zones

before remeshing the face zones.

You can also draw the edge zones to determine their direction (that is, the start point and the end

point).

You can modify the node distribution on the edge zones using the Feature Modify dialog box (opened

using the Feature Modify... button in the Surface Retriangulation dialog box). If you want to assign

different node distributions to two or more portions of an edge zone, you can separate the zone based

on a specified feature angle between consecutive edges. Separation is performed automatically at

multiply-connected nodes.

After creating edge zones using an appropriate combination of the edge zone creation approach and

angle criteria, modify the edge zone as required. You can modify the edge zones using the options

available in the Feature Modify dialog box. Refer to Using the Feature Modify Dialog Box (p. ) for

details on using the various options available in the Feature Modify dialog box.

It is also possible to modify the edges of the zones using the operations in the Modify Boundary

dialog box. Any edges you create must have the same direction as the edge zone.

Important

You cannot remesh a continuous edge zone. You must first separate it into two or more

non-continuous edge zones (that is, edge zones with start and end points).

If the mesh resolution on the boundary face zone is not enough, or you want to create triangular faces

on a boundary face zone that currently has quadrilateral faces, you can remesh that boundary face

zone. You can remesh the boundary face zone using the Surface Retriangulation dialog box (see

Using the Surface Retriangulation Dialog Box (p. ) for details).

Remeshing Boundary Zones

The generalized procedure for remeshing a boundary face zone using the Surface Retriangulation

dialog box is as follows:

.

Create the edge zones as appropriate.

a.

Select the boundary face zone for which you want to create edge zones in the Boundary Face

Zones selection list.

b.

Select the appropriate option from the Angle Criterion drop-down list.

By default, the Face Zone approach is used to create edge zones. Therefore, you can only

specify the required Angle Criterion in the Surface Retriangulation dialog box. If however,

you want to use Face Seed approach, you can use the Feature Modify dialog box to create

the edge zones instead (see Creating Edge Zones (p. )).

c.

The edge zones created will now be available in the Edge Zones selection list.

c.

d.

Select the appropriate zones in the Edge Zones selection list and click Draw to display them.

The selected edge zones will be displayed in the graphics window. If you are not satisfied

with the edge zones and you want to modify them, open the Feature Modify dialog box.

.

Modify the edge zones as required using the options available in the Feature Modify dialog box. Click

the Feature Modify... button to open the Feature Modify dialog box. Refer to Modifying Edge

Zones (p. ) for details.

When you are satisfied with the edge zones you can proceed to remesh the faces.

.

Select the zone to be remeshed in the Boundary Face Zones list.

You can select only a single boundary face zone for remeshing, unless the Use Conformal Remesh

option is enabled.

.

Set the appropriate remeshing options in the Face Remesh Options group box.

a.

Enable Size Field if you want to use the size field to remesh the faces.

Note

Edge zones associated with face zones are not remeshed implicitly. If you have

feature edge zones associated with the surface being remeshed, you need to

remesh them before remeshing the face zones.

b.

Select the appropriate options from the Reconstruction (Order) drop-down list in the Face Remesh

Options group box.

c.

Enable Replace Face Zone, if required.

Important

Remeshing can be performed on both triangular and quadrilateral face zones.

However, it will always result in a triangular face zone.

d.

Enable Use Conformal Remesh if you want to conformally remesh multiple face zones connected

along the shared boundary.

Note

d.

Note

This option is available only when Size Field is enabled and None is selected in the

Reconstruction drop-down list.You will be asked to compute the size field or read a

size field file.

Periodic face zones cannot be remeshed using this option.

Set the minimum Corner Angle to specify the minimum angle between feature edges that

will be preserved during remeshing.

Note

The shared boundary between different zones will be remeshed only if all the

face zones incident to it are selected for conformal remeshing.

.

Click Remesh to remesh the face zones.

Note

Edge zones are saved when the mesh file is written.

You can repair surfaces having internal cracks or free edges using the Faceted Stitch option. You can

specify an appropriate tolerance value within which the free edges will be stitched. The Self Stitch only

option allows you to stitch the edges within the same boundary zone. The faceted stitching operation

is available only for triangular boundaries.

Figure . : Mesh (A) Before and (B) After Using the Faceted Stitch Option (p. ) shows the repair of

a surface with internal cracks.

Faceted Stitching of Boundary Zones

Figure . : Mesh (A) Before and (B) After Using the Faceted Stitch Option

The command /boundary/remesh/faceted-stitch-zones enables you to perform the faceted

stitching of zones.

Note

Features may not be maintained when using the faceted stitching operation.

Some operations like intersection, joining, stitching, and wrapping are available only to triangular

boundary zones. You can remesh a quadrilateral face zone with triangular faces as shown in Fig-

ure . : Triangulating a Boundary Zone (p. ).

You can use the Triangulate Zones dialog box to perform this operation. The dialog box includes an

option to either copy the quad zones and triangulate the copied zones or replace the original quad

zones with the triangulated zone.

You can also use the command /boundary/remesh/triangulate to perform this operation.

Figure . : Triangulating a Boundary Zone

There are several methods available that allow you to separate a single boundary face zone into multiple

zones of the same type. If your mesh contains a zone that you want to break up into smaller portions,

you can make use of these options. For example, if you created a single wall zone when generating the

mesh for a duct, but you want to generate different mesh shapes on specific portions of the wall, you

will need to break that wall zone into two or more wall zones.

... Separating Face Zones using Hotkeys

... Using the Separate Face Zones dialog box

You can use the hotkey Ctrl+Shift+S to separate faces or zones based on what has been selected. If

help text display is active, a description of the face zone separation options is displayed.

If a multi-region face zone is selected, separation will be by region.

If a single-region face zone is selected, separation will be by angle.The angle may be set using the Separate

Face Zones dialog box.

If a face (or edge) is selected, the face zone (edge zone) separation will be by seed.

If edge zone with face seed selection, then the face zone is separated by edge zone.

If no other selection, separation will be by marked faces.

Faces are marked using the hotkey Ctrl+Shift+J and the mouse probe/face selection filter. If help

text display is active, a description of the marking options is displayed.

Ctrl+S marks individually selected faces.

Ctrl+D marks areas by flood-filling.

Ctrl+R marks areas by adding rings around the selected face.

Ctrl+Q marks faces by quality.

Ctrl+G marks faces by angle relative to the selected face, on the entire face zone.

Ctrl+L marks unmarked island faces.

Separating Boundary Zones

Ctrl+U unmarks selected/all faces.

Ctrl+I opens a dialog box to set options for marking faces.

There are six methods available for separating a boundary face zone using the Separate Face Zones

dialog box accessed via Boundary > Zone > Separate.... They are:

Separating Using Angle

For geometries with sharp corners, it is often easy to separate face zones based on the significant

angle. Faces with normal vectors that differ by an angle greater than or equal to the specified angle

value will be placed in different zones.

For example, if the mesh consists of a cube, and all  sides of the cube are in a single wall zone, you

would specify a significant angle of °. Because the normal vector for each cube side differs by °

from the normals of its adjacent sides, each of the  sides will be placed in a different wall zone.

Separating Using Regions

You can also separate face zones based on contiguous regions. For example, if you want to generate

the mesh in different regions of the domain using different meshing parameters, you may need to

split up a boundary zone that encompasses more than one of these regions. Separating based on region

splits non-contiguous boundary face zones (that is, zones that are separated into two or more isolated

groups) into multiple zones.

This command will also split zones that are divided by another face zone. An example could be two

face zones touching in a “T". Using this command on the top zone (for example, wall- in Fig-

ure . : Face Separation Based on Region (p. )) would split it into two zones. However, individual

faces in the corners at the “T" junction may be put in their own zones. To check for this problem, list

the new face zones (using the List button in the Boundary Zones dialog box), looking for zones with

a single face in them. You can then merge these faces into the appropriate zone.

Figure . : Face Separation Based on Region

Separating Based on Neighboring Cell Zones

Region separation will split wall- in Figure . : Face Separation Based on Region (p. ) into two

zones regardless of whether the two regions are in the same cell zone. However, neighbor-based

separation will yield different results. If both regions are in the same cell zone, wall- will not be sep-

arated (see Figure . : Face Separation Based on Cell Neighbor (p. )). If they are in different cell

zones, the zone will be separated. Thus, when neighbor separation is used, wall- will be separated

only if it is adjacent to more than one cell zone. If the two regions are in two different cell zones, then

wall- has two different neighboring cell zones and therefore it will be separated into two wall zones.

Figure . : Face Separation Based on Cell Neighbor

Separating Based on the Face/Element Shape

You can also separate face zones based on the shape of the faces. For example, if a face zone contains

both triangular and quadrilateral faces, you can separate the zone into two zones (one containing the

triangular faces, and the other containing the quadrilateral faces).

Separating Using a Seed Element

You can separate face zones by specifying a face element (in the face zone) as a seed face. You can

also separate different faces of a single face zone using this method. The surface on which you define

a seed face gets separated from rest of the face zone. You can separate face zones using the seed face

based on the following criteria:

Feature Angle Criteria

This method enables you to separate the surface on which you have defined a seed face from the

surfaces around it based on the specified value of the feature angle. The feature angle is the angle

between the normal vectors of the cells. To separate the face zones based on this criteria, do the

following:

.

Select Seed in the Options list and Angle in the Flood Fill Options list.

.

Specify the seed element in the Face Seed text entry field. Right-click the face you want to choose as

a seed element in the graphics window.The Face Seed field will be updated automatically.

.

Specify the required feature angle in the Angle field.

.

Click Separate.

The surface on which you defined the seed face will be separated from other surfaces of the zone

.

.

for which the feature angle change is greater than or equal to the specified value. For example, if

the mesh consists of a cube, and all  sides of the cube are in a single wall zone, specify a significant

angle of ° and specify a seed face on any one of the walls. Because the normal vector for each

cube side differs by ° from the normals of its adjacent sides, the face on which you have defined

a seed cell will be placed in a different wall zone. Therefore, two zones will be created, one zone

will have a face on which you defined a seed face and the second zone will have remaining faces.

Edge Zone Criteria

This method enables you to separate the surface, on which you have defined a seed face, from the

other faces in the zone based on the existing edge zones associated with it. You must create the

edge zones for the given mesh to use this method.

To separate the face zones based on this criteria, do the following:

.

Select Seed in the Options list and Edge Loop in the Flood Fill Options list.

.

Specify the seed element in the Face Seed text entry field.

For this method, you will only specify the seed element. The Angle field will not be available.

.

Important

Create edge threads on the surface zones again using the Surface Retriangulation dialog

box after performing above operations.

Separating Based on Marked Faces

You can separate face zones by placing marked faces in a new zone. To use this option in the Separate

Face Zones dialog box, explicitly define a subregion of the domain (using the Boundary Refinement

Region dialog box), then separate face zones based on whether or not each face in the specified zone

is in the selected local region.

Another mesh refinement method involves projecting the nodes of one face zone onto another (possibly

non-planar) face zone to create a new face zone that has the same connectivity as the original face

zone. This new face zone is created after the projection, and no cell zones are created. The face zone

that is projected is not modified in any way.

Projecting a face zone is used mainly to fill in gaps by extending the domain through the projection.

The original connectivity is maintained after the projection, with the effect being that elements on the

connected side zones will be stretched to cover the projection distance. Affected side zones should

then be remeshed to obtain regular size elements on them. Such a remeshing results in a new side

zone, after which you can (and should) delete the original side zone. Finally, you can mesh the domain

to get the volume elements.

You can create groups of faces and edges that will be available in all the dialog boxes along with the

default groups (for example, boundary, tri, quad, and so on). The face and edge zones are grouped

separately. The User Defined Groups dialog box enables you to define new face and/or edge groups,

update existing groups, activate or delete a particular group. Although the dialog box is opened from

the Boundary menu, it can be used with all dialog boxes that contain zone lists.

Note

When a user-defined group is activated, the wild-cards used for zone selection in all the

Note

text commands will return zones contained in the active group. For example, the com-

mand /display/boundary-grid * will display all the boundary zones contained

in the active group.

For object based meshing (see Object-Based Surface Meshing (p. )), you can create a face group and

an edge group comprising the face zones and edge zones included in the specified objects using the

options in the Zone Group group box in the Operations tab in the Manage Objects dialog box. Addi-

tionally, a face zone group is automatically created when a mesh object is created using the Sew oper-

Creating Groups

ation. This face zone group is prefixed by _mesh_group, and enables easy selection of mesh object

For CutCell meshing, the mesher separates the face zones by cell neighbor and creates a face zone

group for the face zones of each fluid cell zone. See Generating the CutCell Mesh (p. ) for details.

Note

Boundary zones are groups of boundary faces. Usually the grouping collects boundary faces with the

same boundary conditions, but further sub-groupings are often used to preserve a sharp edge in the

surface mesh or simply as an artifact of the boundary mesh generation process.

Each zone has a unique ID, which must be a positive integer. You can use the options in the Manage

Face Zones dialog box to manipulate the face zones. find information about each zone, identify them,

merge zones or delete them, change the boundary type of all faces in a zone, rename zones, and rotate,

scale, or translate zones.

Click List to obtain information about the selected face zones.The zone ID, name, boundary type, and

number of faces by type (tri or quad) will be reported.

Use the Change Type option to change the boundary type of the selected face zones.

Note

When changing the boundary type of any zone to type interior, ensure that there is

a single cell zone across the interior boundary. Retaining multiple cell zones across an

interior boundary can cause undesirable results with further tet meshing or smoothing

operations.

Also, face zones having no/one neighboring cell zone should not be changed to type

interior.

The mesh check will issue a warning if multiple cell zones are maintained across an in-

terior boundary. The boundary type in such cases should be set to internal instead.

Use the Copy option to copy the nodes and faces of the selected face zones.

Use the Delete option to delete the selected face zones.You can optionally delete the nodes of the face

zones as well (enabled by default).

Use the Merge option to merge the selected face zones based on Alphabetical Order (default) or Larger

Area.

Use the Rename option to rename the selected face zones.You can optionally change the zone name prefix

as well.

Note

The zone name can have a maximum of  characters.

as well.

Note

Use the Flip Normals option to flip the direction of all face normals on the selected face zones.

Use the Orient option to consistently orient the face normals on the selected face zones.

Use the Rotate option to rotate all nodes of the selected face zones through the angle specified. Enter the

pivot and axis of rotation or use the Define option to select six nodes or positions to define the pivot and

axis instead.You can optionally create a copy instead of replacing the original zones.

Use the Scale option to scale all nodes of the selected face zones by the scale factors specified.You can

optionally create a copy instead of replacing the original zones.

Use the Translate option to translate all nodes of the selected face zones by the translation offsets specified.

Use the Define option to select two nodes or positions to define the translation vector instead.You can

The hotkey Ctrl+Shift+N opens the Change Zone Properties dialog box which enables you to quickly

rename the selected zone, set the boundary type, and set the geometry recovery option (low or high).

Note

When changing the boundary type of any zone to type interior, ensure that there is a

single cell zone across the interior boundary. Retaining multiple cell zones across an

Also, face zones having no/one neighboring cell zone should not be changed to type in-

terior.

The mesh check will issue a warning if multiple cell zones are maintained across an interior

terior.

boundary. The boundary type in such cases should be set to internal instead.

Case files read in the meshing mode also contain the boundary and cell zone conditions along with

the mesh information. The Boundary Conditions dialog box enables you to copy or clear boundary

conditions assigned to the boundary zones when a case file is read.

You can copy the boundary conditions from the zone selected in the With list to those selected in the

Without list using the Copy option.

You can clear the boundary conditions assigned to the zones selected in the With list using the Clear option.

Manipulating Boundary Conditions

You can create specific types of surfaces within the existing geometry using one of the options available

in the Boundary/Create menu.

The Construct Geometry tool (

) also enables you to create a bounding box or cylinder/frustum

for selected or all zones displayed in the graphics window.

The following sections explain how to create surfaces.

... Creating a Bounding Box

... Creating a Planar Surface Mesh

... Creating a Cylinder/Frustum

... Creating a Swept Surface

... Creating a Revolved Surface

... Creating Periodic Boundaries

In some cases, you may want to create a box that encloses the input geometry (for example, creating

a wind tunnel around the geometry). You can create a bounding box around the input geometry or

only the selected zones of the geometry using the Bounding Box dialog box, or the Construct Geo-

metry tool. You can also specify the required clearance values of the bounding box from the bound-

aries of the geometry.

There are two methods available for creating bounding box:

Using Absolute Values

This method enables you to create the bounding box by specifying the minimum and maximum extents

of the bounding box in X, Y, and Z directions.

Using Relative Values

This method enables you to create the bounding box by specifying the relative coordinate values with

reference to the selected face zone.

.... Using the Bounding Box Dialog Box

The procedure for creating a bounding box is as follows:

.

Select the zones around which you want to create a bounding box in the Face Zones list.

.

Select the appropriate method in the Method list.

a.

For the Absolute method, specify the bounding box extents (X Min, X Max, Y Min, Y Max, Z Min,

and Z Max). If you click Compute, the extents will be computed such that the bounding box encloses

the selected boundary zones.

b.

For the Relative method, specify the clearance values in the Delta entry fields (Delta X Min, Delta

X Max, Delta Y Min, Delta Y Max, Delta Z Min, and Delta Z Max).

Initially, all the Delta entry fields will be set to . This implies that the bounding box will

touch the boundaries of the selected face zones. Positive delta values indicate that the

bounding box will be created outside the initial bounding box while negative values indicate

that the bounding box will be created inside the initial bounding box.

.

.

Specify an appropriate value for Edge Length.When you click Compute for the Absolute method, the

value will be automatically set to /10th that of the minimum length of the bounding box.

.

Enable Create Object if you need to create a geometry object based on the bounding box face zone

created.

Note

Do not use the Create Object option if the box is to be used as a body of influence

while setting up the size functions.

.

Click Draw to visualize the bounding box.

.

Click Create to create a bounding box based on the specified parameters.

.... Using the Construct Geometry Tool

) enables you to create a bounding box for selected or all zones

displayed in the graphics window. The bounding box extents are computed based on the entities

selected or displayed and are indicated in the graphics window.

.

Select the zones (if required) and click the Bounding Box tool (

) to preview the bounding box

extents.The bounding box is always created in the global X-Y-Z axes.

.

The bounding box extents can be altered interactively by selecting the direction and dragging the

mouse to change the box dimensions. Click the yellow dot on the bounding box surface to select the

direction.

.

Click Create (

) to open the Create Object dialog box.

a.

Enter an appropriate Object Name.

b.

Specify the mesh size for the surface mesh. By default, the edge length is computed as one fifth

of the smallest side. Alternatively, enable Specify Sizing and specify the size to be used. Click

Preview to visualize the size set.

.

.

Click Create to create the bounding box. A geometry object comprising the bounding box face zones

will be created.

Creating Surfaces

In some cases, you may need to create a plane surface mesh in the geometry (for example, creating

a baffle-like surface inside a hollow tube). You can create a plane surface and mesh the surface using

triangular faces of the required size using the Plane Surface dialog box.

Warning

It is possible to create a planar surface only of rectangular shape; you cannot create a

planar surface of any other shape.

There are two methods available for creating planar surface mesh:

Axis Direction Method:

This method enables you to create the plane surface perpendicular to any of the coordinate axes.

Select the axis perpendicular to which you want to create a planar surface mesh and then, specify

the coordinates of the points that will form a rectangular surface perpendicular to the axis selected.

You can also create a plane surface enclosing the boundaries of the selected face zone using this

method.

Planar Points Method:

This method enables you to create a plane surface mesh from three points in the geometry selected

using the mouse.

The concept of the planar points method is shown in Figure . : Planar Points Method (p. ).

After specifying the planar points, the first point (P1) and second point (P2) are connected to each

other by a line (line-). Another line (line-) is drawn through the third point (P3) parallel to the

first line. Perpendiculars are drawn from points P1 and P3 on line- and line- respectively.

Figure . : Planar Points Method

This creates a rectangular surface that you can mesh as required.

.... Using the Plane Surface Dialog Box

The procedure for creating a surface mesh is as follows:

.

Select the appropriate method in the Options list.

a.

For the Axis Direction method, select the appropriate face zones, direction, and specify the co-

ordinates of the points perpendicular to the axis.

If you select X Axis then the entry box for specifying coordinates in X direction will not be

accessible. This applies to the other two axes as well.

b.

For the Points method, specify the coordinates for the three points defining the plane.You can

click the Select Points... button and select the points using the mouse button.

.

Specify an appropriate value for Edge Length. If you click Compute, the Edge Length will be computed

as /10th of the minimum distance along the coordinate axes.

.

Enable Create Object if you need to create a geometry object based on the plane surface face zone

created.

.

Click Draw to visualize the surface.

.

Click Create to create the planar surface.

In some cases, you may want to create a cylinder or frustum within the existing geometry (for example,

creating an MRF zone for problems involving moving parts such as rotating blades or impellers, creating

a cylindrical surface to close a gap in the geometry, and so on). You can create a cylindrical surface

and mesh it with a triangular surface mesh using the options available in the Cylinder dialog box, or

the Construct Geometry tool.

Using  Arc Nodes: You can create a cylindrical surface using three nodes that lie on a circular arc (see

Figure . : Cylinder Defined by  Arc Nodes, Radial Gap, and Axial Delta (p. )). Specify the radial gap

and taper angle that will determine the actual radii of the cylinder/frustum to be created.You can specify

a positive or negative radial gap value depending on the required size of the cylinder/frustum. A taper

angle of zero will result in a cylinder.The axial delta values determine the axial length of the cylinder/frustum.

The Caps option enables you to create the circular capping surfaces along with the cylindrical surface.

Figure . : Cylinder Defined by  Arc Nodes, Radial Gap, and Axial Delta

Using  Arc Nodes and a Height Node: You can create a cylindrical surface using three nodes which lie

on a circular arc, and a fourth node to determine the height of the cylinder/frustum (see Figure . : Cyl-

inder Defined by  Arc Nodes and a Height Node (p. )).The radii, height, and taper angle will be determ-

ined based on the nodes selected.

Note

A planar annular surface will be created if the four nodes selected are in the same plane

(that is, the height is zero).

Figure . : Cylinder Defined by  Arc Nodes and a Height Node

Using  Axis Locations or  Axis Nodes: You can also create a cylindrical surface by specifying the radii

(r1, r2) of the cylinder/frustum and two points (P1 and P2) defining the axis (see Figure . : Cylinder

Defined by Axial Points and Radii (p. )). Equal values of r1 and r2 will result in a cylinder.The axis can be

defined by specifying the location (X,Y, Z) of the points or by specifying the appropriate boundary nodes

corresponding to the axial points P1 and P2.The Caps option enables you to create the circular capping

surfaces along with the cylindrical surface.

Figure . : Cylinder Defined by Axial Points and Radii

.... Using the Cylinder Dialog Box

The procedure for creating a cylindrical surface is as follows:

.

Select the appropriate option for defining the cylinder.

a.

For the  Arc Nodes method, select the nodes on the circular arc. Enter appropriate values for

Axial Delta , Axial Delta , Taper Angle, and Radial Gap.

b.

For the  Arc,  Height Node method, select the  nodes on the circular arc and the height node.

c.

For the  Axis Locations and  Axis Nodes methods, specify the points defining the axis.You can

specify the locations (or node IDs) manually. Alternatively, you can click the Select Points... (or

the Select Nodes...) button and select the points using the mouse. Enter appropriate values for

Radius1 and Radius2.

.

.

Enable Caps to create the circular capping surfaces along with the cylindrical surface.

.

Enable Create Object if you need to create a geometry object based on the cylinder/frustum face zones

created.

Note

Do not use the Create Object option if the cylinder/frustum is to be used as a body

of influence while setting up the size functions.

.

Click Preview to preview the cylinder to be created.

.

.

.

When you are satisfied with the settings, click Create to create the cylindrical surface. Enter an appro-

priate zone name prefix in the Object/Zone Prefix dialog box and click OK.

) enables you to create a cylinder/frustum based on selections

in the graphics window. The cylinder/frustum dimensions are computed based on the entities selected

or displayed and are indicated in the graphics window.

.

Select the entities and click the Cylinder tool (

) to preview the cylinder extents. Alternatively,

click the Frustum tool (

) to preview the frustum extents.

When no selections are made, the cylinder/frustum is aligned along the global Z-axis.The default

height and radius are computed based on the bounding box dimensions for the entities displayed.

When face zones are selected, the cylinder/frustum is aligned along the global Z- axis. If any two di-

mensions of the bounding box for the selected zones are the same, the cylinder/frustum will be

aligned along the third (remaining) direction.The default height and radius are computed based on

the bounding box dimensions for the zones selected.

When a single node is selected, it is used as an axis node.The cylinder/frustum will be aligned along

the global Z- axis.The default radius and height are equal and computed as one-tenth the length of

the diagonal of the bounding box for the displayed zones. If no zones are displayed, a value one-

tenth the length of the diagonal of the global bounding box will be used.

When two nodes are selected, the mid-point of the line joining the two is used as an axis node and

the cylinder/frustum will be aligned along the global Z-axis. If the nodes selected are aligned in the

Z-axis, the cylinder/frustum will be aligned along the global Y-axis instead.The default radius and

height are equal, and computed as half the distance between the selected nodes.

When three nodes are selected, the cylinder/frustum base circle passes through the selected nodes.

The axial direction is determined by the right hand thumb rule.The default radius and height are

equal.The radius is determined by the nodes selected.

When four nodes are selected, the first three are used to determine the cylinder/frustum base circle.

The fourth node is used to determine the height.The radius is determined by the first three nodes

selected.

.

The cylinder dimensions can be altered interactively by selecting the direction and dragging the mouse

to change the dimensions. Click the yellow dot on the cylinder surface to change the height.

The frustum dimensions can be altered interactively by selecting the direction and dragging the

mouse to change the dimensions. Click the yellow dot on either surface to change the radii and

height.

.

a.

b.

Specify the mesh size for the surface mesh. By default, the edge length is computed as one-seventh

the average radius or height, whichever is smaller. Alternatively, enable Specify Sizing and specify

the size to be used. Click Preview to visualize the size set.

c.

The Caps option enables you to create the circular capping surfaces along with the cylindrical

surface. Disable this option to obtain only the cylindrical surface.

.

Click Create to create the cylinder/frustum. A geometry object comprising the cylinder/frustum face

zones will be created.

In some cases, you may want to create a swept surface by projecting an edge zone along a specified

linear distance in a specified direction. You can create a swept surface using the options available in

the Swept Surface dialog box.

.... Using the Swept Surface Dialog Box

The procedure for creating a swept surface is as follows:

.

Create the edge zone for the swept surface.

Use the interactive edge zone creation tool to extract edge zones from existing face zones or surfaces.

See Extract Edge Zones (p. ) for details.

Use the Loop Selection tool to create an edge zone from selected nodes or points. See Using the

Loop Selection Tool (p. ) for details.

Use edge zone creation and modification options available in the Manage Objects, Feature Modify,

or Surface Retriangularization dialog boxes. See Object Manipulation Operations (p. ), Using the

Feature Modify Dialog Box (p. ), or Using the Surface Retriangulation Dialog Box (p. ) respectively.

.

Open the Swept Surface dialog box.

Boundary → Create → Swept Surface...

.

Select the edge zone to be swept from the Edge Zones drop-down list.

.

Select the corresponding faces from the Face Zones selection list.

.

.

.

.

Specify the distance along which the edge is to be swept in the Total Distance field.

.

Specify the appropriate value in the No. of Offsets field.

.

Specify the Vector defining the direction in which the edge is to be swept.

Alternatively, you can click Define and select two nodes or positions to specify the vector. The

Total Distance is also computed based on the nodes/positions selected.

.

Enable Split Quad Faces, if required.

.

Enable Create Object if you need to create a geometry object based on the swept surface face zone

created.

. Click Create to create the swept surface.

In some cases, you may want to create a revolved surface from specific edge zones. The revolved surface

is created by revolving the selected edge zones through the angle specified using the pivot and axis

of rotation defined. You can create a revolved surface using the options available in the Revolved

Surface dialog box.

.... Using the Revolved Surface Dialog Box

The procedure for creating a revolved surface is as follows:

.

Create the edge zones to be used for creating the revolved surface.

.

Open the Revolved Surface dialog box.

Boundary → Create → Revolved Surface...

.

Select the edges to be revolved from the Edge Zones selection list.

.

Specify the appropriate value in the Number of Segments field.

.

Specify the angle through which the edge is to be revolved in the Angle field.

.

Specify an appropriate value for Scale Factor depending on the radius required for the revolved surface.

.

Specify the pivot point and the axis of revolution. Click Define and select - nodes to define the pivot

and axis as follows:

If only  node is selected, the pivot point is at the node location and the axis of rotation is the global

z-axis.

For  nodes, the pivot point is at the midpoint of the nodes selected and the axis of rotation is the

For  nodes, the pivot point is at the first node selected.The axis of rotation is the local z-axis normal

For ,  or  nodes, the first  points define a circle.The pivot point is at the center of the circle.The

axis of rotation is the local z-axis normal to the circular plane, the positive direction is determined by

the right-hand rule.

.

Enable Create Object if you need to create a geometry object based on the revolved surface face zone

created.

.

Click Create to create the revolved surface.

.

created.

.

Use the Make Periodic Boundaries dialog box to Create or Recover the periodic relationship between

master and shadow face zones in a single mesh object. The periodic boundaries are identical and

contain either face or node correspondence information.

The Make Periodic Boundaries dialog box is accessible using the context sensitive menu under any

mesh object or using the Boundary  → Create → Periodic... menu.

Create Periodic Boundaries

You can Create new periodic boundaries using the following procedure.

.

In the preprocessor, create only one of the boundaries which is to be made periodic.The to-be-periodic

boundary may have multiple face zones, but should be any non-periodic boundary type.

.

In the Make Periodic Boundaries dialog box in Fluent meshing, select the boundary zone(s) from the

Boundary Zones list.You can also select the zone(s) graphically; the names will be highlighted in the

Boundary Zones list.

.

Enter, or check for accuracy, the periodicity information (angle, pivot and axis for rotational periodicity;

shift vector for translational periodicity) in the Make Periodic Boundaries dialog box.

Periodicity information may be defined graphically (see below) or using the context-sensitive

menu under Model in the Outline View, or read in with the mesh file.

.

A corresponding periodic shadow boundary will be added to the object. A zone type of periodic

will be assigned to both the periodic and the periodic-shadow zones, and the face/node corres-

pondence will be generated.

Important

Important

This is the only way to create periodic boundaries in the meshing mode; it is not sufficient to

simply set a zone type to be periodic.

Periodicity information will be stored with the mesh data and will be extracted when the mesh

file is read. Multiple periodicities may be created, but only the first is read automatically with

the mesh data.

To define periodicity information by other means, follow these steps.

For rotational periodicity, the pivot point and axis of rotation can be defined graphically by selecting -

nodes as follows, and then clicking Define.

– If only  node is selected, the pivot point is at the node location and the axis of rotation is the global z-

axis.

– For  nodes, the pivot point is at the first node selected.The axis of rotation is the local z-axis normal to

the plane defined by the three points, the positive direction is determined by the right-hand rule.

– For ,  or  nodes, the first  points define a circle.The pivot point is at the center of the circle.The axis

of rotation is the local z-axis normal to the circular plane.The x-axis (°) is defined by the 4th, 5th and

6th points and the positive direction is determined by the right-hand rule.

For translational periodicity, the shift vector can be defined graphically clicking Define and then selecting

two nodes.

Rotational periodicity information may be set using the Periodicity dialog box accessed by right clicking

on Model in the Outline View.

two nodes.

Rotational periodicity information may be set using the text command boundary/set-periodicity.

When the periodic-shadow boundary is created from the original (periodic) boundary, the nodes around

the outer edges of the shadow zone will be duplicates of existing nodes. These duplicates will be

marked as free, so they can be verified by counting them and drawing them. Before generating the

initial mesh, you must merge these nodes.

Important

To ensure that the periodic-shadow boundary creation works properly, you must define the

node distribution correctly in the preprocessor that generates the boundary mesh.

Ensure that the distribution of nodes on the boundaries that will be shared by the shadow zone and

the surfaces adjacent to it is the same as the distribution on the boundaries shared by the original

(periodic) zone and its adjacent surfaces.

Note

Files created prior to Release  written in mesher mode are automatically converted when

read into mesher mode. These files may not contain sufficient information to properly set

up periodic information in case of multiple periodic pairs.

Recover Periodic Boundaries

You can Recover periodic boundaries if it exists from a mesh file using the following procedure.

.

Read the mesh file.

.

In the Make Periodic Boundaries dialog box in Fluent meshing, select the periodic boundary zone(s)

from the Boundary Zones list.

Tip

You can also select the zone(s) graphically, and the names will be highlighted in the

.

If it exists, periodic information (angle, pivot, and origin) will be extracted from the mesh file when

.

it is read and will appear in the Periodicity dialog box. Alternatively, you can manually enter

periodic information as described above.

.

Click Recover.

The Recover feature will check for any existing face zone(s) at the periodic shadow boundary. If

a shadow face zone is more complex than the corresponding master, the recover operation will

fail for that zone and a warning will appear in the console. You may be able to recover the peri-

odic boundary by reversing the angle and selecting the more complex face zone(s).

Note

Recover first creates the periodic shadow boundary and then removes any duplicate face zone(s)

at the periodic shadow boundary.

Periodic boundary recovery may be initiated using the text command boundary/recover-

periodic-surfaces.

Use the Remove Boundary Gaps dialog box to remove gaps between boundary zones.

.

Select the target zone in the graphics window. Click

to set the target zone.

.

Select the zones for the gap removal operation and click

to open the Remove Boundary Gaps

dialog box. Alternatively, select the zones and use the hot-key Ctrl+K.

.

.

.

.

.

in the graphics window or using the hot-key

Ctrl+Shift+L. This tool provides options for creating an open or closed loop of nodes. You can create

an edge zone or capping surface based on the loop selected. You can also select positions instead of

nodes to define the loop.

Figure . : Loop Selection Toolbar

loop.

The second group of icons is used to select open or closed loop.Then, for closed loop mode, you can choose

how the path between the first and last nodes is defined - by edges, feature, boundary, or direct path.

Creating a Capping Surface

(hot-key Ctrl+K) in the Loop Selection mode to open

the Create Cap dialog box. The Create Cap dialog box contains options for object/zone granularity

and type and for remeshing the capping surface.

.

Using the Loop Selection Tool

.

.

Creating an Edge Zone

(hot-key Ctrl+L) in the Loop Selection mode to open

the Create Edge Zones dialog box. The Create Edge Zones dialog box enables you to add the edge

zone to an existing object or create an unreferenced edge zone.

Selecting all Nodes

(hot-key Ctrl+J) in the Loop Selection mode to select

all the nodes on the loop. These selections can then be used for operations such as collapsing, merging,

or smoothing nodes.

Chapter :Wrapping Objects

Geometries migrated from various CAD packages often contain gaps and overlaps between the surfaces

due to algorithm and tolerance differences of the CAD packages. Repairing such geometries manually

is a tedious and time-consuming process. Wrapping provides the ability to create reliable meshes for

such geometries without extensive manual clean up and reduces the time required for preprocessing.

The object wrapping operation:

extracts a conformal, well connected mesh object on the relevant surfaces of the objects selected.

can repair gaps and overlaps in the model at the expense of a user-specified degree of geometry details.

can handle unclean geometries and does not require a watertight representation of the geometry.

can be used for defeaturing or when you need to walk over features.

The wrapper is useful in the following industrial applications:

Automotive

– Underhood thermal management (engine only, front car, full car)

– Cabin HVAC

– External aerodynamics

– Brake cooling and engine cooling

Aerospace

– Engine core compartment

– Cockpit HVAC, cabin HVAC

– Landing gear

Drill bit applications

Smoke and fire spread

Biomedical applications

Other applications with bad input geometries

..The Wrapping Process

The wrapping operation uses an appropriate material point to identify the relevant surfaces of the se-

lected objects. A well-connected mesh object is created.

The general procedure for creating a wrapper surface is as follows:

. A coarse Cartesian grid is overlaid on the selected objects (including gaps and overlaps) to create a con-

tiguous region.This Cartesian grid is used to automatically clean the input geometry and to create the

water-tight representation.

. The Cartesian grid is then refined based on the size functions to better represent the selected objects.

. The intersection between the Cartesian grid and the input geometry is calculated and the intersecting cells

are identified and marked.

. The interface is extracted on the boundary of the non-intersecting Cartesian volume region that encloses

the material point. A watertight, faceted representation is created along the boundary of the intersecting

cells.

cells.

. The nodes on this faceted representation are projected onto the faces and feature edges of the input

geometry which then results in a wrapper surface closely representing the input geometry.The edges are

imprinted on the wrapped zones, and individual zones are recovered and rezoned based on the original

. The wrapper surface quality is improved by post-wrapping operations such as smoothing, swapping, and

so on. Degenerate and island edges are deleted, and intersected and remeshed as appropriate. Surfaces

are remeshed based on size functions/size field.

Figure . : Schematic Representation of Wrapping Process (p. ) is a simple illustration of these steps.

Figure . : Schematic Representation of Wrapping Process

Note

If the global minimum size specified cannot be resolved, an error will be reported. Set up appro-

priate sizes and compute the size field before wrapping.

Wrapping Objects

If the minimum and maximum sizes from the size field cannot be resolved, increase the

minimum size and recompute the size field before wrapping.

The wrapping operation approximates the geometry using a stairstep-like Cartesian grid without

projection. It requires finer cells to resolve thin gaps.

In cases when a gap area is curved and not aligned to the Cartesian axes, you may need

to refine – times finer than the gap thickness. This should be taken into account while

setting the global and local minimum size for size functions and the cells per gap for the

proximity size function being used.

You may specify a Resolution Factor to allow finer cells without changing the size function.

The dimensions of the distortion (for example hole, gap, and so on) in the input geometry should

be smaller than that of the size of the Cartesian cells created by the wrapper. If there is significant

distortion in the input geometry, repair it to the extent that the distortion becomes smaller in

size. Large holes, if present in the initial geometry, should be filled. Otherwise such holes will be

ignored in the wrapping process.

The object wrapping utility is accessed using the context sensitive menus. Right click on any object and

select Wrap. The following sections discuss tools and options used in the wrapping process.

Note

The Improve... option is available only for mesh objects.

... Extract Edge Zones

... Create Intersection Loops

... Setting Geometry Recovery Options

... Fixing Holes in Objects

... Shrink Wrapping the Objects

... Improving the Mesh Objects

... Object Wrapping Options

You can easily extract edge zones from existing face zones or selected surfaces using context menus

from the tree or onscreen tools. In either case, edge zones are created using the Fixed Angle criterion

as described in Creating Edge Zones (p. )

The Wrapping Process

Using Onscreen Tools

You can use the onscreen tools to create edge zones interactively on selected face zones or selected

surfaces. This method has the advantage of previewing any edges that meet the specified criteria before

creating the edge zones.

. Set the required Selection Filter.

Use Face Selection Filter to create edge zones on the surface(s) that contain the selected face(s).

Use Zone Selection Filter to create edge zones on the selected face zone(s).

. Using the mouse probe, select the face(s) or face zone(s) for which edge zones are to be created.

. Click the Create Edge Zones tool button (

).

If a zone is selected, the Interactive Edge Zone Creation dialog box opens.

If a face is selected, the Create Edge Zones By seed dialog box opens.

Any edges on the selected surface, or face zone, that meet the dihedral angle criterion will be

highlighted.

. Adjust the Preview Edge Angle slider as necessary to select the edge threads to be included in the

new edge zone, based on the Fixed Angle criterion.

. Click Create Edge Zones.

The new edge zone will be added to the object that contains the selected face (or face zone).

Using Context Menus

You can use the context menus to extract edge zones for any selected geometry or mesh object in

the tree.

. In the Outline View, select the geometry object or mesh object.

. Right-click on the selected object, and select Wrap → Extract Edges....

Note

This option is also available under the Advanced menu.

. Specify the threshold Angle.

From the Option list, choose whether feature or all edges are to be extracted.

. Click OK.

The extracted edge zones are placed in the Unreferenced branch of the tree.

Note

The Extract Edges dialog box offers the same functionality as the Edge Zones group on the

Operations tab of the Manage Objects dialog box. See Object Manipulation Operations (p. ).

The Feature Modify and Surface Retriangularization dialog boxes also contain groups to

modify or create Edge Zones. See Creating and Modifying Features (p. ) or Remeshing

You can use these options to choose how face zones are processed within objects, prior to wrapping.

.... Individually

Within each object, edge zones are created on the loops where the face zones overlap. In Figure . : In-

dividual Object Loop (p. ), after applying Create Intersection Loops → Individually to all objects,

only one such edge zone is created - in the large geometry object at the intersection of the two cubic

volumes.

Figure . : Individual Object Loop

.... Collectively

Edge zones are created on the loops where face zones overlap, both within a single object and

between multiple objects. In Figure . : Collective Object Loops (p. ), an additional edge zone is

created where the large geometry object intersects the smaller object.

Figure . : Collective Object Loops

You can determine the surfaces and features which need to be captured with higher accuracy based

on the usage of the model. For example, when using a car model for an external aerodynamic simulation,

the recovery of external surfaces requires greater accuracy. Other components like the braking system

or underhood components can be recovered with lower accuracy since they are not as significant for

the simulation.

The recovery of features and surface mesh quality are controlled by setting the Geometry Recovery

attribute for objects or face zones in the Geometry Recovery Options dialog box. The wrapped surface

mesh inherits the geometry recovery attribute from the underlying objects or face zones.

Low

enables you to create a rough wrapped representation of the selected objects. Features are not preserved

and the mesh quality is not as good as a CFD mesh.

High

enables better feature capture and high quality surface mesh. By default, the High attribute is set for all

face zones in the mesh.

To set the geometry recovery attribute,

. Right-click on any geometry or mesh object, and then select Wrap → Geometry Recovery Options...

to open the Geometry Recovery Options dialog box.

. Select the objects or face zones in the selection list.

. Click Apply for the appropriate option in the Geometry Recovery group box.

To visualize the geometry recovery option, use the hot key Ctrl+Shift+C to go to Color Options Mode,

then Ctrl+G to apply color by geometry recovery.

The region/volume of interest should be well connected before the volume mesh can be generated.

Any holes or leaks need to be located and fixed before proceeding with volume meshing. Holes/leaks

can be located using a material point. When you select the material point and set the minimum and

maximum limits for the hole size, those locations, within the set size limits, at which a path traces back

to the material point through the geometry are recognized as holes or leaks.

When you refine an existing region or specify additional sizing functions for better representation of

the geometry, the minimum size may be reduced to a size smaller than some existing leakages. These

leakages can be detected automatically using the automatic hole detection tool in ANSYS Fluent

Meshing. The refinement of a region may result in the joining of previously separate regions through

cells newly introduced by the refinement (region collision). While refining a region, ANSYS Fluent

Meshing will automatically detect cells causing region collision and group them. Such groups of cells

will be identified as holes in the region. The number of holes exposed by the current refinement will

be reported in the console.

The following operations allow you to automatically detect holes:

Refining a single region.

Specifying local size function and additional zone-specific sizes after initialization.

Refining local regions defined according to requirements.

You can use the Fix Holes dialog box to locate and fix such holes as described in the following generic

procedure:

.

Right-click on the selected geometry or mesh object(s) in the Model tree and then select Wrap → Fix

Holes....

You can add or change Objects using the selection list in the dialog box. Click Draw to display

only the selected object(s) in the graphics window.

.

Select an appropriate material point.

The default material point (external) is a suitable point, external to the selected objects. Click

Change to enable the Material Point drop-down list, if necessary.

.

Retain the Use Size Field option, if required.

This will use a size field based on previously defined size controls or size functions to determine

the limits for hole sizes.

a.

Set a Resolution Factor if desired.

Setting a value less than  can help to find holes not aligned to the Cartesian axes by using

a.

finer sampling than the given size field.

In situations where a hole's minimum size is larger than the size field's minimum size, using

a Resolution Factor helps to find holes without modifying the size field. That is, you can use

the same size field for both hole fixing and wrapping.

b.

Set the minimum and maximum limits for the Hole Sizes under consideration.

The size values enable you to limit the search for holes to a relevant subset based on the

size range. As you locate the respective holes and fix them, the possibility of false holes is

reduced.

You can click Draw Sizes to check the sizes on the geometry; click Draw to turn off size

display.

In situations where a hole's minimum size is larger than the size field's minimum size, using the

Resolution Factor helps to find holes without modifying the size field. That is, you can use the

same size field for both hole fixing and wrapping.

You can alternatively choose to use a specific size to find the holes or leaks in the mesh.

To find holes based on a specified size, disable Use Size Field. Enter an appropriate value for Min

Size and click Apply.

The Max Size can be set to limit the search to a relevant size range.

.

Click Find Holes to locate all the holes based on the specified parameters.

The number of holes is reported in the Count field in the Wetted Holes group box.

Using the Pan Regions Dialog Box

The options in the Pan Regions dialog box enable you to observe and analyze the region to be

wrapped, overlayed on a plane aligned with the Cartesian grid. The plane can be passed through the

selected region (or all available regions) along the X, Y, or Z direction, as required. The interior of the

selected region(s) is displayed on the plane, at every position of the plane. Click Pan Regions... to

open the Pan Regions dialog box.

You can also overlay the boundary surfaces while panning, and clip the boundary surfaces on either

side of the cutting plane.

To pan through all the regions of your choice, do the following:

.

Display the required region (using the Draw button below the Regions list).

.

Click the Pan Regions... button to open the Pan Regions dialog box.

.

Select the appropriate axis along which you want to pan through the selected regions from the Direction

list.

The Start, End, and Increment fields will be updated automatically based on the cell size distri-

bution of the Cartesian grid. You can change these values as appropriate.

.

Enable Overlay Graphics if you want to see the geometry along with the pan plane.

Select Positive or Negative to clip the surfaces on the positive or negative side of the cutting

plane. Figure . : Overlaid Geometry Clipped with the Pan Plane (p. ) shows the geometry on

the positive side of the cutting plane.

Figure . : Overlaid Geometry Clipped with the Pan Plane

.

Select the regions to be analyzed in the Region selection list. By default, all regions are selected. In cases

comprising a large number of Cartesian regions, you can pan through selected regions instead.

.

Click Pan to start the plane movement through the selected regions.

.

Alternatively, use the arrow buttons or the slider to manually move the pan plane to a particular

location.

The interior of the Cartesian grid is displayed on every position of the plane during its movement

through the region. Increase (or decrease) the Increment value to increase (or decrease) the speed

of movement of the plane.

Figure . : Leak Detection Using the Pan Regions Dialog Box (p. ) shows how the leakage can

be detected using the Pan Regions dialog box. If, at any position of the plane, the color of the

region is seen inside the geometry, there may be a leak or hole in the Cartesian grid.

Figure . : Leak Detection Using the Pan Regions Dialog Box

.

Adjust the plane at the position where the leak is seen on the plane.

Warning

The Pan Regions dialog box only enables you to know whether or not there is a leak

or hole in the geometry. If the geometry has a hole or leak, you need to find its exact

location and fill it.

Closing holes

Options for closing or opening the holes are in the Operations group box:

You use the Wetted Holes group box to traverse the holes detected, or to globally patch or open all the

holes.

– Click Draw All to view all the wetted holes detected.

– Click First to view the first hole.The display will be limited to the region of the hole.

Click Next repeatedly to traverse all the wetted holes and examine them individually.

– Click Patch All to automatically patch all the wetted holes detected.

– Click Open All to open all the wetted holes detected (when the holes identified do not represent actual

holes).

holes).

You use the Selected Holes or Create Patch group box to close the displayed hole individually.

– Click Patch to automatically close the currently displayed hole.

– Click Open if the currently displayed hole does not represent an actual hole. Opening a hole enables

you to indicate that the approximated wetted region should propagate through the configuration de-

tected as a hole.

– Click Ignore if the currently displayed hole is not relevant for the object wrapping/sewing operation.

– Click Cylinder... to open the Cylinder (p. ) dialog box to create a cylindrical surface to fix the hole.

You use the Trace to Points group box to locate holes or leaks by tracing a path from the Material Point

to a selected Target Point through all the objects. Even after you fix the holes/leaks, you can use the Trace

to Points options to verify that no tiny leaks remain.

.

Select a point from the Target Points selection list and click Trace.

The path connecting the target point to the material point will be highlighted and will pass

through the hole/leak.

.

Fix the hole using the options in the Wetted Holes, Selected Holes, or Create Patch group box, as

appropriate.

.

Click Update in the Wetted Surface group box to update the wetted surface representation.

.

Click Update in the Trace to Points group box and then click Trace again to locate any remaining

holes/leaks.

.

Repeat the hole fixing steps as needed to ensure no holes/leaks remain.

You use the options in the Wetted Surface group box to view the approximate representation of the

.

volume or region of interest based on the objects and material point selected.You can also create a mesh

object using the shrink-wrap method.

– Click Show to view the approximate representation of the wetted surface, based on the objects and

material point selected. Enable Overlay Graphics to view the object(s) along with the wetted surface.

Click Hide to hide the wetted surface in the graphics window.

– Click Update to update the wetted surface representation after any hole fixing operations (patch, open,

creating caps, and so on) are performed.

Examine the updated region for further leaks or holes. Fill any remaining leaks or holes before

After all the holes/leaks are fixed you can proceed to wrap the objects. Specify an appropriate New

Object Name and New Label Name (if required). Click Shrink Wrap to create a mesh object for the

selected objects using the shrink-wrap method.

Important

The octree refinement used to identify and repair holes occurs in a different order than

when used to wrap objects. Thus, using this button may generate a different mesh than if

you use the Wrap dialog box as described in Shrink Wrapping the Objects (p. )

The Wrap dialog box contains options for shrink wrapping the selected objects. Select the objects to

be wrapped in the Outline View and then select Wrap → Shrink Wrap... from the context sensitive

menu to open the Wrap dialog box.

.

Select the appropriate option, Individually or Collectively, from the Target list.These options are de-

.

scribed in Creating Individual Mesh Objects (p. ) and Creating a Collective Mesh Object (p. ).

Creating Individual Mesh Objects

The Individually option enables you to create a conformal surface mesh for each object selected.

A well-connected mesh object and corresponding zones will be created for each object. The mesh

object name is the original object name with the suffix -mesh. This operation uses a suitable

material point that is external to the objects selected. Hence, any internal voids or features will

be eliminated. The mesh objects created are suitable for repair operations such as gap or thickness

removal, or as the final surface mesh.

Figure . : Wrapping Individual Objects (p. ) shows the mesh objects created for geometry

objects using the Individually option.

Figure . : Wrapping Individual Objects

Creating a Collective Mesh Object

The Collectively option enables you to create a single, well-connected mesh object and corres-

ponding zones, based on the objects selected. You can specify an appropriate name for the mesh

object and a new label name.

When you select external in the Material Point drop-down list, a suitable reference point external

to the objects is selected for the object wrapping operation. Hence, any internal voids or features

will be eliminated. Figure . : Multiple Solids (p. ) shows an example with multiple solid objects.

The aim of the object wrapping operation is to mesh the solids conformally and create a single

solid cell zone in the final mesh. Figure . : Single Solid Surface (p. ) shows the mesh object

created, where the multiple solids are unified.

Figure . : Multiple Solids

Figure . : Single Solid Surface

Alternatively, you can use this option to create the flow volume, when the surrounding solids are

not needed in the final mesh. All objects bounding the flow volume should be selected for the

wrapping operation. Select the appropriate material point needed to identify the “wetted” region

that is the flow volume. The material point can be defined in the Material Points dialog box.

Figure . : Extracting the Flow Volume (p. ) shows the extraction of the internal flow volume

for a T-junction by specifying a material point and using the Fluid Surface option.

Figure . : Extracting the Flow Volume

For the Collectively option, specify the New Object Name and New Label Name.

.

Set the Resolution Factor.This field can be used to set sampling coarser or finer than the final surface

mesh.

Tip

For industrial size problems where the geometry recovery is set to high, it is recommen-

ded that the resolution factor not be smaller than ..

Important

Wrapping models with a large number of face zones may cause significant slow down in

performance. Merging face zones with the same boundary conditions will improve the effi-

ciency of the wrapping operation.

Important

When wrapping large, complex geometries with small mesh sizes, you may need to increase

the memory allocation. From the Display → Controls menu, select Shrink Wrap in the

Categories drop down list, and specify a new value for Max Octree Memory.

Important

By default, the initial bounding box for shrink wrapping is the global bounding box. In

Important

multiple session wrapping, a newly created wrapper surface may increase the global

bounding box, which affects subsequent wrapper results. To avoid this issue, go to the

Display+Controls menu, select Shrink Wrap in the Categories drop down list, and choose

selection for the Initial Bounding Box.

You can use the command /objects/wrap/wrap to create the mesh object. Specify the objects

to be wrapped and other relevant parameters.

The command /objects/wrap/set/shrink-wrap-rezone-parameters enables you to set

the parameters for improving the mesh object surface quality using rezoning. The geometry object

zones will be separated based on the separation angle specified to improve the feature imprinting on

the mesh object.

The options in the Improve dialog box enable you to improve the surface mesh quality of mesh objects.

The wrapper surface created after imprinting is of good quality and it represents the input geometry

very well in most regions. However, you can improve it further in some regions of the geometry such

as sharp corners and curves. The post wrapping improvement operations allow you to improve the

wrapper surface by performing various operations such as smoothing, swapping, inflating thin regions,

removing crossovers, and so on.

.

Select the mesh objects in the Outline View. Right-click and select Wrap → Improve... from the context

.

Choose the appropriate Method.

The Smooth and Improve option improves the mesh by a combination of smoothing, swapping, and

.

surface mesh improvement operations. Object normals are correctly oriented and island faces are also

deleted.You can optionally coarsen the surface mesh by specifying a suitable Coarsening Factor.

Additional Imprint operations can be done to improve feature capture on the surface mesh.

Note

Using the Imprint option may result in quality deterioration.

The Surface Remesh option improves the mesh by remeshing based on the current size field. Object

normals are correctly oriented and island faces are also deleted.

.

Set Coarsening Factor and Imprint as desired.

The wrapper surface created may be finer than you require in some regions. You can coarsen the

mesh in such regions or globally for the entire wrapper surface. This operation also reduces the

cell count of the mesh, thereby reducing the computation time.

.

Click Improve.

Note

Additional controls can be set in the Objects category in the Display → Controls dialog

box for improving the mesh object quality.

Enable the Improve Quality Aggressively option to collapse faces without preserving

boundary features. This option is disabled by default.

You can alternatively use the command /objects/improve-object-quality.

The following object wrapping options are available:

.... Resolving Thin Regions During Object Wrapping

.... Detecting Holes in the Object

.... Improving Feature Capture For Mesh Objects

during the object wrapping operation and surface elements may span between nodes on the prox-

imal surfaces.

You can use the command /objects/wrap/set/include-thin-cut-edges-and-faces to

enable better recovery of such configurations during the object wrapping operation.

The command /objects/wrap/set/report-holes? enables you to check for holes in the object

created. Holes, if any will be reported at the end of the object wrapping operation.

The command /objects/wrap/set/max-free-edges-for-hole-patching enables you

to set the maximum number of free edges in a loop to fill the holes.

The command /objects/wrap/check-holes enables you to check for holes in the objects. The

number of hole faces marked will be reported.

The command /objects/improve-feature-capture enables you to imprint the edges com-

prising the mesh object on to the object face zones to improve feature capture for mesh objects. You

can specify the number of imprinting iterations to be performed.

Note

The geometry objects used to create the mesh object should be available when the im-

prove-feature-capture command is invoked. Additionally, the face zones comprising

the objects should be of type other than geometry.

Chapter : Creating a Mesh

After reading the boundary mesh and performing the necessary modifications (such as merging duplicate

nodes, edge swapping) you will create the volume mesh.

Depending on the type of mesh you are starting from (boundary mesh only, boundary mesh with

hexahedral cells in one or more regions, and so on), you can automatically generate the mesh, manually

generate the mesh step by step, or use a combination of manual and automatic commands.

You can create several types of meshes comprising different element types. The meshing strategy and

the use of the Auto Mesh tool are described in this chapter. Information on how to deal with thin regions,

quad-tet transition elements (pyramid and non-conformal meshing), and creation of a heat exchanger

zone are also described. Detailed descriptions of meshing techniques such as prism meshing, tetrahedral

and hexcore meshing options, and so on are described in subsequent chapters.

.. Choosing the Meshing Strategy

.. Using the Auto Mesh Dialog Box

.. Generating a Thin Volume Mesh

.. Generating Pyramids

.. Creating a Non-Conformal Interface

.. Creating a Heat Exchanger Zone

.. Parallel Meshing

You can use a variety of cell shapes to mesh the domain:

Figure . : Possible Mesh Cell Shapes

A mesh consisting entirely of tetrahedral elements is a tetrahedral mesh, and a mesh with any combin-

ation of cell shapes is referred to as a hybrid mesh.

Before generating a volume mesh, determine the shapes that are appropriate for the case you are

solving, then follow the instructions for creating the required cell types. Most cases will fall into one of

the following categories:

... Boundary Mesh Containing Only Triangular Faces

... Mixed Boundary Mesh

... Hexcore Mesh

... CutCell Mesh

... Additional Meshing Tasks

... Inserting Isolated Nodes into a Tet Mesh

If you require a high mesh resolution in some portion of the domain, such as a boundary layer, you

can obtain an efficient and better quality mesh by meshing that portion with prisms (wedges) and

then meshing the rest of the domain with tetrahedra (tets). The resulting mesh is referred to as a viscous

hybrid mesh.

The procedure is as follows:

Creating a Mesh

. Build one or more layers of prisms, starting from the appropriate boundary (or boundaries). Refer to

Generating Prisms (p. ) for details.

. Create a domain encompassing the region to be meshed with tetrahedra. Refer to Using Domains to

Group and Mesh Boundary Faces (p. ) for details.

. Generate the tets in the selected domain using either an automatic tet mesh generation, a manual tet

mesh generation, or a combination of the two. Refer to Generating Tetrahedral Meshes (p. ) for details.

Figure . : Mesh with Prisms in a Boundary Layer Region (p. ) shows several layers of prisms in a

portion of a mesh created in this manner. The prisms extend throughout the entire region bounded

by the quadrilateral faces, but only a few of them are shown here.

Figure . : Mesh with Prisms in a Boundary Layer Region

The surface mesh originally contained only triangular faces. The quadrilateral faces are created auto-

matically when the prisms are built on the triangular faces.

If the quadrilateral faces of the prisms do not lie on the external boundary of the domain (that is, if

the prism region begins and/or ends in the interior of the domain), create a layer of transitional pyr-

amids between steps  and . Refer to Generating Pyramids (p. ) for details.

If you have no special boundary layer resolution requirements, you can generate a mesh consisting

entirely of tetrahedra (see Figure . : Surface Mesh Containing Only Tetrahedra (p. )). You can use

the automatic tetrahedral mesh generation procedure, the manual procedure, or a combination of

both. Refer to Generating Tetrahedral Meshes (p. ) for details.

Figure . : Surface Mesh Containing Only Tetrahedra

Start from a boundary mesh that contains triangular and quadrilateral faces as well as hexahedral cells

in the quadrilateral face regions. The resulting mesh is referred to as a zonal hybrid mesh.

. Add a layer of pyramids to the quadrilateral boundary face zone that lies between the hexahedral region

and the adjacent region to be meshed with tetrahedra.This creates the triangular boundary face zone

that is required to create tetrahedra in the adjacent region. Refer to Generating Pyramids (p. ) for details.

. Generate the tetrahedra in the selected domain using either automatic or manual tet mesh generation,

or a combination of both. Refer to Generating Tetrahedral Meshes (p. ) for details.

Figure . : Surface Mesh (p. ) shows the surface mesh for a portion of a grid containing hexahedra,

pyramids, tetrahedra, and prisms that was created on a plenum feeding a valve-port cylinder.

Figure . : Surface Mesh

Choosing the Meshing Strategy

The less complicated plenum pipe on the left of the figure is meshed using hexahedral cells.

The more complex valve port (valve not visible because it is inside the surrounding pipe) is meshed using

tetrahedra.

Pyramids are used as a transition between the hexahedral grid for the plenum and the tetrahedral grid for

the valve port.This transition occurs where the triangular and quadrilateral faces meet in the middle of

the figure.

Additionally, the quadrilateral faces produced by extending triangular faces in the cylinder (that is, the

quadrilateral sides of the resulting prism wedges) can be seen in the far right of the figure.

The hexcore mesh features a tetrahedral/hybrid mesh adjacent to walls and a Cartesian mesh in the

core flow region. Figure . : Hexcore Mesh (p. ) shows the typical hexcore mesh. The hexcore

meshing scheme creates a mesh consisting of two regions:

An inner region composed of regular Cartesian cells.

An outer region consisting of tetrahedral elements.

Figure . : Hexcore Mesh

Wedge elements are created only when boundary layers are attached on faces pre-meshed with trian-

gular elements. It combines the automation and geometric flexibility of tetrahedral/hybrid meshes

with greatly reduced cell counts in many applications. The hexcore mesh is most beneficial in geometries

with large open spaces, as in automotive, aerospace, and HVAC applications. Refer to Generating the

Hexcore Mesh (p. ) for details.

CutCell meshing is a general-purpose hex-dominant meshing technique that can be used instead of

tetrahedral or hexcore meshing, without requiring a very high-quality surface mesh as a starting point.

This method uses a direct surface and volume approach without the need of cleanup or decomposition,

thereby reducing the turnaround time required for meshing. A key feature is the large fraction of hex

cells in the mesh.

Figure . : CutCell Mesh

Refer to Generating the CutCell Mesh (p. ) for details.

Additional meshing tasks that can be handled are:

If you have a complete volume mesh and want to extend some portion of the domain (for example, increase

the length of an inlet pipe), you can grow one or more layers of prisms from the current external (quadri-

lateral or triangular) boundary.

Figure . : Extending an Existing Tetrahedral Mesh Using Prisms (p. ) shows a region of prisms

(wedges) extended from the triangular face zone that bounds a tetrahedral region.

Figure . : Extending an Existing Tetrahedral Mesh Using Prisms

Unless there is a reason to use hexahedral cells in the quad regions, it is preferable to convert a mixed

tri/quad boundary mesh to an all-tri boundary mesh and then create a tetrahedral mesh for a 3D boundary

mesh consisting of only triangular faces.

Use the Triangulate Zones dialog box or the command /boundary/remesh/triangulate to

convert quad face zones to tri face zones.

You can then use the Boundary Improve dialog box to improve the skewness of the triangular

boundary zone created.

You may choose to use a non-conformal interface to define the computational domain.This type of interface

enables you to relax the requirement for point-to-point matching at the interface between the meshes, as

illustrated in Figure . : Example of a Non-Conformal Interface (p. ).

Figure . : Example of a Non-Conformal Interface

This feature of relaxing the requirement for point-to-point matching at the interface between the

meshes is particularly useful in parametric studies where you want to change an isolated region of

the domain without changing the entire mesh. The procedure is as follows:

. Read the meshes in meshing mode in Fluent.These meshes need not share nodes, edges, faces, or cells.

. Create the volume mesh using an appropriate meshing strategy.You can also create domains for each

independent mesh region and mesh the individual domains separately.

. Separate the region of non-conformal interface into new face zones. Use Boundary → Manage to

change the face zone type of the two surfaces that will be treated as non-conformal to interface.

. Transfer the mesh to solution mode in Fluent and create the non-conformal interface using the Mesh

Interfaces dialog box. Refer to Mesh Interfaces Dialog Box (p. ) for details.

To add nodes to the mesh without specifying the faces, you can create a boundary zone in the

boundary mesh (in the program that created it) just for this purpose, then you can introduce the nodes

associated with these faces.

This feature is useful for clustering nodes (and therefore cells) in a controlled manner. Figure . : Mesh

Generated Using Isolated Nodes to Concentrate Cells (p. ) shows a mesh that was generated using

this method to cluster the nodes behind the wedge. A mesh that was generated for the same geometry

without clustering is shown in Figure . : Mesh Generated Without Using Isolated Nodes (p. ).

You can follow either of the two procedures to insert isolated nodes into a mesh:

Delete the face zone before meshing.

Introduce the nodes using face zones after meshing.

Deleting the Face Zone Before Meshing

This procedure is as follows:

.

Delete the face zone, but leave the associated nodes. Disable Delete Nodes in the Manage Face Zones

dialog box to retain these nodes.

Note

By default, the unused nodes are deleted when the faces of the zone are deleted.

.

Disable Delete Unused Nodes in the Tet dialog box and generate the volume mesh.

Note

By default, unused nodes will be deleted during the automatic meshing.

The nodes will be introduced when you initialize the mesh. When you use this procedure, all

nodes must be inserted into the mesh or the initialization will fail.

Warning

Do not place isolated nodes too close to the boundary or to other nodes.

Figure . : Mesh Generated Using Isolated Nodes to Concentrate Cells

Figure . : Mesh Generated Without Using Isolated Nodes

Introducing the Nodes Using Face Zones After Meshing

.

Create a subdomain that does not include the face zones used to control the mesh density.

.

.

.

Create the volume mesh using the subdomain.

.

Activate the global domain.

.

Introduce the additional nodes using the text command: /mesh/modify/mesh-nodes-on-zone.

Important

The /mesh/modify/mesh-nodes-on-zone command will delete the faces associ-

ated with the face zone.

The Auto Mesh dialog box enables you to automatically create the volume mesh using the different

mesh elements available. This dialog box can used for generating the volume mesh based on face zones

or based on a mesh object and relevant material points. For more detail about object-based mesh

generation, refer to Objects (p. ).

The generic procedure for using the Auto Mesh dialog box for creating the volume mesh is as follows:

.

Determine the meshing approach (face zone based or object based) and the mesh elements required for

the particular case.

.

Open the Auto Mesh dialog box using the Mesh → Auto Mesh... menu item or from the context-sensitive

menu available by right-clicking on any Mesh Object, or its Cell Zones or Volumetric Regions branch

in the Outline View.

.

Select the appropriate option in the Object drop-down list in the Auto Identify Volume group box.

a.

For the face zone based meshing approach, ensure that none is selected in the Object drop-down

list.

b.

For the object based meshing approach, select the appropriate mesh object in the Object drop-down

list. Enable/disable Keep Solid Cell Zones and Keep Dead Cell Zones as required.

Tip

If you open the Auto Mesh dialog box from the context-sensitive menu in the

Tip

Model tree, the Mesh Object is automatically selected.

.

box.

Using the Auto Mesh Dialog Box

a.

approach.

b.

Select scoped if you want to specify object-specific prism parameters. Click Set... to open the Scoped

Prisms dialog box and define the prism parameters and scope. Refer to Prism Meshing Options for

Scoped Prisms (p. ) for details.

c.

.

Select the appropriate quad-tet transition elements from the Quad Tet Transition list. Click Set... to open

the Pyramids dialog box or the Non Conformals dialog box (depending on the selection) and specify

the appropriate parameters. Refer to Creating Pyramids (p. ) and Creating a Non-Conformal Inter-

face (p. ) for details.

.

Select the appropriate option from the Volume Fill list. Click Set... to open the Tet, Hexcore, or Poly

dialog box (depending on the selection) and specify the appropriate parameters. Refer to Initializing the

Tetrahedral Mesh (p. ), Refining the Tetrahedral Mesh (p. ), Controlling Hexcore Parameters (p. ),

and Steps for Creating the Polyhedral Mesh (p. ) for details.

Note

The No Fill option is not available for object based volume meshing.

.

a.

Note

.

a.

b.

c.

For the Poly-Hexcore method, set the following:

Specify the number of Buffer Layers and Peel Layers.

Specify the Min Cell Length for the poly-hexcore approach.

The hybrid poly-hexcore volume meshing method is a combination of the existing poly and

the octree hexcore meshing algorithms, and is available for serial processing only, with object

based workflows when the Grow Prisms option is set to none or scoped.

While similar to the Octree mesh option, the Poly-Hexcore option leverages the use of hexcore

volume meshing and uses a polyhedron transitional mesh rather than a tetrahedron transitional

mesh.

.

mesh.

.

For object-based meshing enable Merge Cell Zones within Regions to create a single cell zone within

a region, or disable to keep the cell zones separate.

For zone-based meshing, enable Merge Cell Zones to create a single cell zone within a domain,

or disable to keep the cell zones separate.

Note

For object-based meshing and parallel processing, after your mesh is distributed, this

option is active automatically.

To apply parallel processing of the mesh, enable Auto Partition (Parallel Meshing). This option

is only available for Poly-Hexcore volume fill (enabled by default), or for zone-based meshing with

Tet and prism volume fill, and is not available for the pure tetrahedra, polyhedra, or hexcore fill

methods. The Auto Partition (Parallel Meshing) option is also only available when the number

of parallel processors is greater than ). Enabling this setting will also enable the Auto partition

option in the Parallel Mesh Settings dialog box (see Auto Partitioning (p. )). Disable the Auto

Partition (Parallel Meshing) option if you are interested in only generating the volume mesh in

serial mode.

.

Click Mesh to automatically create the mesh.

Note

text commands prior to using the auto-mesh command.

Thin Volume Mesh creates sweep-like mesh for a body occupying a thin gap. You define boundary

face zones for source and target such that the source face normal should point to the target. The source

face mesh may be triangles or quads. Four other controls are then used by Fluent Meshing to grow the

volume mesh from the source zone to the target zone.

To generate a Thin Volume Mesh:

.

Check the source boundary mesh to ensure that free nodes or faces with high skewness do not exist. See

Manipulating Boundary Nodes (p. ) and Determining Surface Mesh Quality (p. ) for details.

.

Open the Thin Volume Mesh dialog box.

Mesh → Thin Volume Mesh

.

Select the Source Boundary Face Zone from the list.

.

Select the Target Boundary Face Zone from the list.

.

Specify the Gap Thickness.

If set to , the mesher will automatically calculate the gap thickness.

If non-zero, the Gap Thickness defines the maximum separation between source and target zones in

the swept-mesh region.

.

Specify the Number of Divisions between source and target faces.

.

Specify the Growth Rate between adjacent layers.

.

.

.

.

Choose Remesh overlap zones behavior. Remesh overlap zones replaces any overlapped part of the

surface mesh on the target and adjacent faces. Original meshes in these areas are replaced.

.

Click Create to calculate the thin solid mesh.

. Click Draw to display the mesh in the graphics window of the user interface.

A pyramid has a quadrilateral face as its base and four triangular faces extending from the sides of the

quadrilateral up to a single point above the base. See Figure . : Pyramid Cell—Transition from a

Hexahedron to a Tetrahedron (p. ).

Figure . : Pyramid Cell—Transition from a Hexahedron to a Tetrahedron

To generate a conformal mesh with a region of tetrahedral cells adjacent to a region of hexahedral

cells, you will first create a layer of pyramids as a transition from quadrilateral faces to triangular faces.

After creating a single layer of pyramids, the resulting triangular faces will be used to create tetrahedra.

To create pyramids, you need to specify the boundary from which the pyramids will be built, the

method for determining the top vertex of each pyramid, and the pyramid height.

... Creating Pyramids

... Zones Created During Pyramid Generation

... Pyramid Meshing Problems

The procedure for creating a layer of pyramids from a quadrilateral boundary zone is as follows:

. Check the aspect ratio limits of the boundary face zones on which you need to build pyramids.

Report → Size Field

The use of a high-aspect-ratio quadrilateral for the base of a pyramid produces skewed triangular

faces that can cause problems during the tetrahedral mesh generation. If the maximum quadrilat-

eral face aspect ratio is much greater than , you will need to regenerate them.

If the faces were created in a different preprocessor, return to that application and try to reduce the

aspect ratio of the faces in question.

If the faces were created during the building of prism layers, rebuild the prisms using a more gradual

growth rate.

. Select the appropriate quadrilateral boundary zones in the Boundary Zones selection list in the Pyramids

Mesh → Pyramids

Click Draw to view the selected zones.

If the quadrilateral zone you require does not appear in the list, use the /boundary/reset-

element-type text command to update the type of the zone. It is possible that the quadrilateral

zone may not be recognized the due to changes made to the boundary mesh.

Generating Pyramids

For example, if you separate a mixed (tri and quad) face zone into a tri face zone and a quad face

zone, each of these will be identified as a mixed zone. You need to reset the element type for the

quad zone for it to be recognized and included in the Boundary Zones selection list.

. Select the appropriate method for determining the pyramid vertex location in the Options list.The

skewness method is selected by default, and is appropriate for most cases.

. Specify the height of the pyramids by setting the Offset Scaling value.

. Click Create.The new pyramid cell zone and the new face zones created will be reported in the console.

You can then use the Display Grid dialog box to view these new zones.

Display → Grid

. Change the boundary type of the quadrilateral base zone to the appropriate type (if necessary).

Boundary → Manage

Note

Because you built cells next to the quadrilateral base zone, its original boundary type

may no longer be correct.

Important

The pyramids should be automatically created on the appropriate side of the specified

boundary zones. If the pyramids are on the wrong side, do the following:

. Delete the newly created zones related to the pyramids.

. Reverse the normal direction on the quadrilateral boundary where the pyramids are being

built (using the Flip Normals option in the Manage Face Zones dialog box).

. Recreate the pyramids.

When pyramids are generated, at least two new zones are created: a cell zone containing the pyramid

cells and a face zone containing the triangular faces of the pyramids.

The following zones will be created during pyramid generation:

The cell zone containing the pyramids (pyramid-cells-n).

The face zone containing the triangular faces of the pyramid cells (base-zone-pyramid-cap-n).

For example, if the pyramids were built from the quadrilateral face zone wall-, they will be placed

in a new zone called wall--pyramid-cap- (where the  is the zone number assigned).

The face zones containing the pyramid sides that use existing faces from the original boundary mesh

(base-zone-pyramid-side:n), where, n is the zone number assigned.

For example, if triangular boundary faces from the zone wall- are used, they will be placed in a

new zone called wall--pyramid-side- (where the  is the zone number assigned).

Important

If you include the pyramid-side boundary zones when defining the domain in which

you are going to generate a tetrahedral mesh, the tetrahedral meshing will fail.

Most problems associated with creating pyramid layers manifest themselves in the subsequent process

of generating the tetrahedral mesh.

Rapid Changes in Volume

Rapid changes in the sizes of cells have a negative influence on the convergence and accuracy of the

numerical solution. The pyramid layer creation can produce rapid variations in cell volume in the fol-

lowing situations:

If the quadrilateral surface mesh has faces with rapid changes in size.

If there is great disparity between the sizes of the quadrilateral faces and the neighboring triangular faces

used in the pyramid creation.

You can avoid the rapid variation in volume by creating quadrilateral and neighboring triangular grids

with smooth variations in face size.

Intersecting Faces

If the quadrilateral surface used to create pyramids has highly concave corners, the resulting pyramids

may pierce each other and/or neighboring boundary faces:

Figure . : Pyramid Cells Intersecting Each Other and Boundary

In such cases, you can either increase the resolution to prevent the intersections or alter the meshing

strategy. An alternative is to separate the quadrilaterals in the concave corner into another zone (using

techniques described in Separating Boundary Zones (p. ) or Modifying the Boundary Mesh (p. )),

create triangular faces from the quadrilateral faces using the /boundary/remesh/triangulate

text command, and then create pyramids.

The skewness-based pyramid creation will use the existing triangular faces and avoid the intersection

problem (see Figure . : Fixed Intersecting Pyramid Cells Using Triangular Faces (p. )).

Figure . : Fixed Intersecting Pyramid Cells Using Triangular Faces

High Aspect Ratio

Creating pyramids on quadrilateral faces with very high aspect ratios results in highly skewed triangular

faces. Subsequent attempts to create a tetrahedral mesh from these elements will produce a poor-

quality mesh.

Irrespective of the method used to generate the quadrilaterals, modify the meshing strategy to reduce

the aspect ratio using an external grid generation package or the prism layer capability.

For meshes containing both hexahedral and tetrahedral elements, you can generate a non-conformal

interface to avoid creating intermediate pyramids as transition elements between the quadrilateral and

triangular surfaces. You can also choose to create a non-conformal interface when growing prisms from

a boundary on a surface mesh, to avoid quad faces in the domain to be meshed. The surfaces containing

quad elements will be copied and then triangulated while keeping the original surfaces intact. The free

nodes of the triangulated surface will then be merged with the nodes on the original surface mesh.

Both surfaces will then be converted to interface type.

The options in the Non Conformals dialog box enable you to create a non-conformal interface.

... Separating the Non-Conformal Interface Between Cell Zones

The command /mesh/non-conformals/separate enables you to separate the face zones at the

non-conformal interface between the cell zones specified. Specify the cell zones where the interface

is not conformal, an appropriate gap distance (absolute or relative), and the critical angle to be used

for separating the face zones. The gap distance used for the separation is the larger value of the absolute

gap distance specified and the relative gap distance times the average local edge length. You can also

choose to orient the boundary face zones after separation and additionally write a journal file during

the separation operation. This journal file can then be read in solution mode to create the mesh inter-

faces automatically.

The separated face zones will be named as follows: cell zone :cell zone -orig face zone  for face

zone  attached to cell zone  and cell zone :cell zone -orig face zone  for face zone  attached

to cell zone . If the separated interface zone has more than one face zone, the original face zone

contributing a larger number of faces will be used for the name.

Invalid contact locations will be skipped during the separation operation. The location of the invalid

contact will be reported in the console.

Many engineering systems, including power plants, climate control, and engine cooling systems typically

contain heat exchangers. However, for most engineering problems, it is impractical to model individual

fins and tubes of the heat exchanger core.

You can create a heat exchanger volume mesh using the options in the Heat Exchanger Mesh dialog

box.

Creating a Heat Exchanger Zone

The heat exchanger mesh created contains prisms generated from a quad split surface mesh. You need

to specify four points (either by selecting the locations or nodes) and the required intervals between

the first selected point and the each of the remaining points to create the heat exchanger mesh. A

meshed plane is created using the first three specified points and the corresponding intervals. Prisms

are created on the meshed plane using the fourth point and the corresponding interval.

Mesh → Create → Heat Exchanger...

.

In the Location group box, select Position or Nodes to specify the source for location coordinates.

.

Click Select Points... or Select Nodes... and select the four points (nodes) in the correct order.

Important

The order of selection of the points is important because the heat exchanger zone is

created based on the intervals specified between the first selected point and each of

the remaining points. If the points are not specified in the correct order, you will get a

heat exchanger zone that is different from the required one.

.

In the Create By group box, select Interval or Size to setup the mesh density.

.

Specify the number of intervals (or mesh size) between selected points (nodes) –, –, and –, respect-

ively.

.

Enable Create Object, if you need to create a mesh object for the heat exchanger mesh zones created.

.

Click Preview to preview the heat exchanger zones and modify the parameters if you are dissatisfied with

the results.

.

.

.

.

Specify the prefix for the zones as required in the Object/Zone Prefix dialog box and click OK.

The heat exchanger zones (prefixed by hxc-) are created as shown in Figure . : Creating the Heat

Exchanger Mesh (p. ).

Figure . : Creating the Heat Exchanger Mesh

If you launched Fluent with parallel processing for meshing enabled, you will be able to distribute the

mesh data across the available compute nodes, or recombine the mesh data as required. For additional

information on specifying parallel processing, see Starting ANSYS Fluent Using Fluent Launcher (p. ).

The following options are available for parallel meshing:

... Auto Partitioning

... Computing Partitions

... Controlling the Threads

Auto partitioning enables automatic decomposition of the mesh into suitable partitions for parallel

meshing. The prism base zones will be automatically partitioned if zone-specific prism parameters or

scoped prism controls are specified. The prism mesh will be generated on the respective compute

nodes. After the prism mesh has been generated, the tetrahedral mesh will be generated on compute

node .

Follow these steps to generate the mesh using auto-partitioning.

. Prepare the surface mesh for volume meshing. Ensure that the mesh quality and connectivity are appro-

priate.

. Enable Auto Partition in the Parallel Mesh Settings dialog box.

When Auto Partition is enabled, and after volume meshing has occurred, several elements of the

graphical user interface are no longer available (Availability of Graphical User Interface Options

After Parallel Meshing (p. )). Likewise, there are elements of the text user interface that are also

no longer available (Availability of Text Interface Options After Parallel Meshing (p. )).

. Create the volume mesh using the options in the Auto Mesh dialog box.

Note

Available volume meshing options include zone-specific or scoped prisms, pyramid and

non-conformal quad-tet transition, and tetrahedral fill.

For object-based meshing, the object backup cannot be created and hence, the mesh object

surface mesh cannot be restored later.

. Improve the volume mesh using the options available, if required.

. Save the mesh or case file.

Note

The case file will be written in HDF5 format and can be read only in Fluent solution

mode.

Parallel Meshing

.... Availability of Graphical User Interface Options After Parallel Meshing

After auto partitioning is enabled, and after parallel meshing has occurred, the following items in the

graphical user interface are not available as noted:

Unavailable Items

Location

Free Face

Display (Ribbon)

Remesh

Patch Options (Ribbon)

Separate

Append File(s)

Select File Dialog

(File > Read Mesh)

Merge Nodes

Boundary Menu

Intersect

Create

Create

Modify Boundary Dialog (Opera-

tions)

Merge

Delete

Collapse

Split

Swap

Prisms

Separate Face Zones  Dialog (Op-

tions)

Thin Volume Mesh

Seed

Flip Normals

Manage Face Zones Dialog (Op-

tions)

Orient

Prisms

Mesh Menu

Pyramids

Non-Conformals

Tet

Hexcore

CutCell

Create

Tet Improve (not available for the Poly- Hexcore

tions)

Orient

Prisms

Mesh Menu

Pyramids

Tet

Hexcore

CutCell

Create

volume fill method, otherwise, available for the Tet

volume fill method using prisms)

Mesh > Tools

Cavity Remesh

Improve (not available for the Poly- Hexcore volume

fill method, otherwise, available for the Tet volume

fill method using prisms)

Mesh > Tools > Prism

Location

Split

Post Ignore

Tet Improve Cavity

Split

Modify Cells Dialog (Options)

Swap

Construction Geometry

Outline View:

Model context menu options

Periodicity

Diagnostics

Model > Geometry Objects

context menu options

Convert to Mesh Object

Wrap

Remesh

Advanced

Model > Mesh Objects context

menu options

Wrap

Remesh Faces

Join/Intersect

Recover Periodic

Restore Faces

Advanced

Model > Mesh Objects > Face

Zone Labels sub-level context

Compute

Model > Mesh Objects > Volu-

metric Regions context menu:

Validate

Update

metric Regions sub-level

Manage

Scoped Prisms

Tet

Hexcore

Location

Graphics Toolbars:

Construct Geometry

Loop Selection Mode

Miscellaneous Portions of the

Context Toolbar

.... Availability of Text Interface Options After Parallel Meshing

text user interface are not available as noted:

Status

Command

TUI Menu

objects/

available

check-mesh

available

delete

available

delete-all

available

delete-all-geom

available

delete-unreferenced-faces-and-

edges

available

extract-edges

available

list

available

merge-walls

available

rename-cell-zone-boundaries-us-

ing-labels

available

rename-object

available

rename-object-zones

available

rotate

available

scale

available

summary

available

translate

available

update

mesh/

not available

auto-mesh-multiple-objects

auto-prefix-cell-zones

available

domains/

manage/auto-set-active

manage/get-material-point

modify/extract-unused-nodes

modify/list-skewed-cells

modify/repair-negative-volume-

cells

not available; available when Auto

Partition is disabled

non-conformals/

available

prepare-for-solve

available

prism/

prism/create

prism/mark-ignore-faces

prism/mark-nonmanifold-nodes

prism/controls/

scoped-prisms/

tet/

boundary/

available

delete-unused-nodes

modify/

When the mesh file is initially loaded, all mesh data is associated with compute node . Compute the

partitions based on the closed regions in the mesh. Each closed region will be assigned to the compute

nodes available with some consideration for load balancing. When the mesh is distributed, the mesh

data will be distributed to the compute nodes based on the partitions computed. Combined mesh

data is required for geometry and surface mesh repair.

Follow these steps to distribute the mesh across the available compute nodes.

. Section the boundary zones.

Any closed surface mesh between objects or bodies may serve to separate sections. The domain

may be pre-partitioned (independent creation of separate regions), or you may take advantage of

regions in the geometry, or you may maintain a surface mesh between objects or bodies.

Parallel meshing supports non-conformally connected bodies if they can be identified as separate

bodies. Within a body, surfaces must be conformal.

. Open the Parallel Mesh Settings dialog box under Parallel → Mesh Settings....

. Click Compute Partitions.

All the Boundary Zones will be assigned to the available partitions as groups of closed regions.

Assignment is based on location with some consideration for load balancing.

If the number of closed regions is less than the number of compute nodes, then the number of

regions is taken as the number of partitions and the other compute nodes will be idle with no

mesh.

. Use the Compute Node Num, List, and Draw controls to examine the expected mesh distribution.

. Click Distribute Mesh.

Mesh data will be distributed to the available compute nodes based on the computed partitions.

Note

If you read in a case file (using the File → Read → Case... menu or the /file/read-

case command) and then distribute the mesh, boundary conditions may not be pre-

served.

Note

served.

. Create your volume mesh.

Note

non-conformal quad-tet transition, and tetrahedral fill. Unavailable options will be greyed

out.

For object-based meshing, any existing object backup data will be deleted and hence, the

mesh object surface mesh cannot be restored later.

If including prism layers, consistent orientation must be done before computing the volume

mesh.

The mesh created by parallel processing is valid although it may have some differences

when compared to a serial processed mesh.

. If necessary to perform geometry or surface mesh repair, use Agglomerate Mesh.

Distributed mesh data will be recombined into a single partition on compute node .

You can control the maximum number of threads on each machine by using the Thread Control

dialog box (Figure . : The Thread Control Dialog Box (p. )).

Parallel → Thread Control...

Figure . : The Thread Control Dialog Box

You have the following options when using the Thread Control dialog box:

Number of Node Processes on Machine

When this option is chosen, the maximum number of threads on each machine is equal to the

number of ANSYS Fluent node processes on each machine.

Number of Cores on Machine

This is the default option. When this option is chosen, the maximum number of threads on each

machine is equal to the number of cores on the machine. ANSYS Fluent obtains the number of cores

from the OS. This may be applicable when the multi-threaded part of the calculation is dominating

the computation time, and the continuous phase calculation is relatively small, and you want to

take full advantage of the computation resources. For example, if you have a very small case with

regard to the number of cells, but a large number of particles to be tracked, you may want to spawn

one ANSYS Fluent node process on each machine, but use the maximum number of cores in order

to get a good overall performance.

Fixed Number

When this option is chosen, you may specify the maximum number of threads that can be spawned

on each machine in the number-entry box below Fixed Number. This may only be applicable when

you want to have fine control of the number of threads on each machine; it is not recommended

in general.

Chapter : Generating Prisms

You can create prism cells starting from either quadrilateral or triangular boundary faces, or both. Prisms

can be used to resolve a boundary layer region of a tetrahedral mesh. They can be used to extend some

portion of a domain for which the volume mesh already exists (for example, increase the length of an

inlet pipe), or to create a volume mesh by extrusion.

Figure . : Prism Shapes (p. ) shows the types of prisms that can be generated.

Figure . : Prism Shapes

To create prisms, you need to specify the surfaces from which the prisms will be built and the parameters

that control the prism growth. Details about how the parameters are used to generate the prisms are

provided in The Prism Generation Process (p. ).

For zone-based prism growth, the prisms are grown from selected boundary zones. Growth parameters

such as offset and growth methods, prism height, the number of layers, and the direction may be applied

only to specific zones. Additional growth options including options for prism proximity detection and

splitting can also be specified. Instructions for building zone-based prisms are provided in Procedure

for Creating Zone-based Prisms (p. ). The additional options are described in Prism Meshing Options

for Zone-Specific Prisms (p. ).

For object-based meshing, use the scoped prism process to select regions for prism creation and set

up controls for the prism generation. Each control specifies the offset method, prism height, number

of layers and growth rate (scoped prism uses the geometric growth method). The scope for prism creation

can be set to fluid-regions, solid-regions, or specifically named-regions. Within the selected regions,

you can grow prism layers on only-walls (default), all-zones, or the solid-fluid-interface. Alternatively,

you can grow prism layers on selected zones (selected-face-zones) or face zone labels (selected-labels).

The scoped prism controls can be read from a previously saved file or can be written to a file for further

use. These options are described in Prism Meshing Options for Scoped Prisms (p. ).

Problems related to prism generation are discussed in Prism Meshing Problems (p. ).

..The Prism Generation Process

The following process is used by the mesher to build the prisms and to create a high-quality mesh.

.

Boundary mesh analysis:

.

The initial surface mesh is analyzed to determine if any adjacent zones should be projected to ad-

jacent zones and retriangulated (if triangular), or if their faces should be used as the sides of new

prism cells (if quadrilateral).

For details on determining whether to use existing boundary zones or not, see Using Adjacent

Zones as the Sides of Prisms (p. ).

.

Prism layer growth.

Prism layers are grown one by one, based on the layer height specification. This is a multistep

procedure, and hence some of the steps may be modified or skipped:

a.

Determine the initial direction vectors so that the direction in which to build the prisms is determined.

The direction methods available are discussed in Direction Vectors (p. ).

b.

Check for proximity and determine shrinkage of prism layers based on the proximity options specified.

c.

Determine the initial offset distances so that the mesher will know how far from the corresponding

nodes on the previous layer to place the new nodes that define the prisms. See Offset Distances (p. )

d.

Smooth the initial direction vectors. See Normal Smoothing (p. ) for details.

e.

Adjust and smooth the offset distances to eliminate spikes and dips in the new prism layer. See Offset

Smoothing (p. ) for details

f.

Project new nodes along the outer edges of the prism layer to adjacent zones, based on the analysis

in step .

g.

Create prism faces and cells using the new nodes.The new faces at the top of the prism layer are

referred to as cap faces.

h.

The new cap faces of skewness value greater than the specified threshold are improved by edge

h.

swapping or edge node smoothing. See Edge Swapping and Smoothing (p. ) for details.

i.

Apply global smoothing across the new surface.This is also skewness-driven, but is based on the

nodes not the faces. See Node Smoothing (p. ) for details.

j.

Check the quality of all new cells and faces.

k.

If quality problems are detected, prism layer creation is stopped. If more layers are to be grown, the

process is repeated starting from substep (a).

.

Zone clean up: After all the prism layers have been grown, the new faces along the outer sides of the

layers are moved to zones of the same types as the zones to which their nodes are projected. Unprojected

faces are collected in a single prism-side zone.

.

Retriangulation: Adjacent triangular zones that have been projected to adjacent zones are automatically

retriangulated.Triangles that are overlapped by new quadrilateral faces from the prism layers are removed.

Most of the original nodes are used in the new triangulation.The result is a conformal interface between

the sides of the prism layers and the adjacent triangular zones.

Generating Prisms

... Zones Created During Prism Generation

When prisms are generated, several new cell and face zones are created. You can identify the new

zones by their default names.

The cell zone containing the prisms will be named prism-cells-#.

The face zone created at the end of the last prism layer will be named prism-cap-#.

If the prism layers are bounded by one or more existing triangular face zones, each of these will be retrian-

gulated so that the faces of the zone that are adjacent to the prisms will become quadrilateral faces, while

the rest of the faces in the zone remain triangles.

If an original triangular face zone is called symmetry, the portion of it that still contains triangles

will be retained as symmetry, while the portion containing quadrilateral faces will be named

symmetry-quad:#.

Any faces that were not projected to adjacent zones (see Using Adjacent Zones as the Sides of Prisms (p. ))

are collected into a zone named prism-side-n.

For a zone wall-#, the zone created by ignoring prism growth in the region of proximity will be named

as wall-#:ignore, where, # is the zone number assigned.

Important

All the ignored threads related to a base thread will be merged into a single thread by

default. You can however change this using the command /mesh/prism/con-

trols/merge-ignored-threads? which will generate more than one thread per

base thread.

To merge one or more prism cell zones with other cell zones (and merge the corresponding face

zones), use the Merge option in the Manage Cell Zones dialog box.

By default, the prism-cap-# zones will be wall zones. If you do not want to include these walls in

the model, change them to interior zones (or any other type) using the Manage Face Zones dialog

box.

Note

If the prism mesh is generated using the Auto Mesh tool and Merge Cell Zones is enabled,

the new face zones will be merged with the original boundary zones and a single cell zone

.. Procedure for Creating Zone-based Prisms

The procedure for creating prisms by setting up zone-specific parameters is as follows:

.

Check the boundary mesh to ensure that free nodes or faces with high skewness do not exist. See Manip-

.

ulating Boundary Nodes (p. ) and Determining Surface Mesh Quality (p. ) for details.

Procedure for Creating Zone-based Prisms

.

Select the boundary zones from which you want to grow prisms in the Boundary Zones selection list in

the Prisms dialog box.

Mesh → Prisms...

Alternatively, when using Auto Mesh, select zone-specific in the Grow Prisms drop-down list and

click Set... to open the Prisms dialog box.

Important

If you read in a mesh file created in a previous version, it is recommended that you reset

all the prism parameters using the command /mesh/prism/reset-parameters

before proceeding with setting the prism parameters.

.

Specify prism growth parameters in the Growth tab.

a.

Select the appropriate Offset Method and Growth Method for growing prisms.

Figure . : Layer Heights Computed Using the Four Growth Methods (p. ) shows layer

heights for all four methods, using a first height of  and a slope/rate/exponent of ..

Figure . : Layer Heights Computed Using the Four Growth Methods

See Offset Distances (p. ) for details.

b.

Define the height of the first prism layer (First Height/First Aspect Ratio).

c.

Set the growth method related parameter (Slope, Rate, or Exponent, as applicable) and the Number

of Layers.

d.

Specify options for prism growth, proximity detection, and splitting of prism layers (if needed) in the

Prisms Growth Options dialog box (opened using the Growth Options... button), if required. Refer

to Prism Meshing Options for Zone-Specific Prisms (p. ) for details.

e.

e.

Click the Plot button to preview the height distribution.

For information on setting different growth parameters for different zones, see Growing Prisms

Simultaneously from Multiple Zones (p. ).

.

Specify the direction for prism growth (see Direction Vectors (p. )).

a.

Click the Direction tab in the Prisms dialog box to view the direction parameters.

b.

Verify the orientation of the normals for the zones on which you want to grow prism layers. Ensure

that the normals are pointing in the direction that you want to build the prisms.

You can use the Color by Normal option, accessible using the hotkey Ctrl+Shift+C then

Ctrl+N to verify the normal direction.

If the boundary zone normals are incorrectly oriented, click the Orient Normals... button to open

the Orient Normals dialog box. Specify the material point based on which the normals are to be

oriented and click Apply.

For mesh objects, use the options in the Orient Mesh Object Face Normals group box to orient

the normals.

a.

Select the mesh object in the Object Name drop-down list.

b.

Select Region or Material Point as appropriate, and then select the region or material point

in the drop-down list.

c.

Ensure that Select is enabled, and enable Select Walls and/or Select Baffles as needed.

d.

Click Orient.

Face boundary zone groups comprising the prism base zones will be created (prefixed

by _prisms).

c.

Specify the method for determining the direction of the prisms:

Select Normal in the Method list to compute normal direction vectors.This method takes into

c.

account the change in direction required for a curved region. Specify the values for the maximum

angle change.

Select Uniform in the Method list to use a constant, uniform direction for flat prism regions.

Specify the appropriate direction vector.

.

Set the parameters for prism improvement and prism projection available in the Improve and Project

tabs, respectively, as required. See Improving Prism Mesh Quality (p. ) or Using Adjacent Zones as the

Sides of Prisms (p. ) for more information.

.

Click Apply to save your settings.

.

Save the mesh:

File → Write → Mesh

Important

It is a good practice to save the mesh at this point. If you are dissatisfied with the prisms

generated, you can read in this mesh and modify the prism parameters to regenerate

the prisms.

.

Click Create to generate only the prism cell zone.

Refer to Prism Meshing Problems (p. ) for suggestions on solving problems occurring during

prism generation.

Alternatively, when using Auto Mesh, click Apply and close the Prisms dialog box. The prism cells

will be created first, and then the mesher will proceed to generating the tet/hexcore mesh. Refer

to Using the Auto Mesh Dialog Box (p. ) for details.

.

Check the maximum face skewness value reported in the console when the final prism layer is created,

to ensure that the value is acceptable.

This is especially important if you are going to generate tetrahedral or pyramidal cells using this

new boundary zone.

The new zone should not have highly skewed triangles or quadrilaterals. For more information

about the quality of quadrilateral faces used for creating pyramids, refer to Creating Pyramids (p. ).

If the reported maximum skewness is too high, read the mesh file you saved after setting the prism

parameters and try again with different parameters. Refer to Prism Meshing Problems (p. ) for

details.

. A number of new zones are created when the prism generation is complete (see Zones Created During

Prism Generation (p. )). If the prism-cap or prism-side face zones are not supposed to be walls (for ex-

ample, if they are supposed to be simple interior zones), change them to the appropriate boundary type.

For most cases, performing these steps will result in an acceptable mesh of prismatic cells, but for some

complex geometries, you may have to modify the procedure. If you are not satisfied with the prisms

generated, you can read in the mesh you saved before generating prisms and modify the prism para-

meters. Refer to subsequent sections for details on modifying the prism generation parameters to create

a better mesh.

The procedure for using zone-specific prism controls for creating prisms during volume meshing using

Auto Mesh is described in Using the Auto Mesh Dialog Box (p. ).

.. Prism Meshing Options for Zone-Specific Prisms

This section describes the prism meshing options available for creating a prism mesh based on zone-

specific settings.

... Growth Options for Zone-Specific Prisms

... Offset Distances

... Direction Vectors

... Using Adjacent Zones as the Sides of Prisms

... Improving Prism Mesh Quality

... Post Prism Mesh Quality Improvement

This section describes the additional growth options available for creating a prism mesh based on

zone-specific settings.

.... Growing Prisms Simultaneously from Multiple Zones

Prism Meshing Options for Zone-Specific Prisms

.... Growing Prisms on a Two-Sided Wall

.... Ignoring Invalid Normals

.... Detecting Proximity and Collision

.... Splitting Prism Layers

.... Preserving Orthogonality

You can select multiple face zones for simultaneously growing prism layers. If the face zones are

connected, the prisms grown will also be connected. A single zone of prism cells and a single zone

of cap faces will be created for each set of simultaneously grown layers. To retain the individual prism

cell zones and cap face zones, enable Grow Individually in the Prisms Growth Options dialog box

(opened by clicking the Growth Options... button).

You can grow prisms from multiple zones with the same or different growth parameters.

To use the same growth parameters for all zones, follow the steps in Procedure for Creating Zone-based

Prisms (p. ). In this case, the same number of layers are grown from all zones, and all other parameters

(growth method, offset method, direction method, and so on) also remain the same.

To use different growth parameters for different zones, you can apply different growth methods, offset

methods, first height, and other growth parameters (as required for the growth method selected) individu-

ally for each zone and click the Apply button in the Zone Specific Growth group box in the Prisms dialog

box.

If you specify different growth parameters for different zones, all other parameters (direction

method, offset method, and so on) can be set separately for each zone. In this case, the offset

height of each node that is shared by multiple zones will be the average of the heights applied on

the separate zones.

This produces a continuous transition between the zones (Figure . : Different Growth Parameters

on Adjacent Zones (p. )). Offset smoothing (see Offset Smoothing (p. )) is recommended in

these cases to avoid sharp height changes at such edges.

Figure . : Different Growth Parameters on Adjacent Zones

To assign different growth controls and different offset types to different face zones, replace steps

and  in Procedure for Creating Zone-based Prisms (p. ) with the following steps:

.

Select the zones for which you want to specify a set of growth parameters in the Boundary Zones

list in the Prisms dialog box.

.

Set the appropriate Offset Method, Growth Method, First Height, and the related growth parameters

(as required) in the Growth tab.

.

Specify parameters for proximity/collision detection in the Prisms Growth Options dialog box (see

Detecting Proximity and Collision (p. ) for details).

Important

By default, a single zone of prism cells and cap faces is generated for the simultan-

eously grown prism layers. If you want to retain individual prism cell zones and cap

faces, enable Grow Individually in the General Options group box in the Prisms

Growth Options dialog box.

.

Click Apply in the Prisms dialog box.

.

Repeat this procedure for other zones for which you want to apply different growth controls.

.

.

.

.

Warning

Before you click the Create button, ensure that all the zones for which you want

to grow prisms are selected in the Boundary Zones list.

Note

When the Prisms dialog box is used to generate prism layers on multiple zones

(adjacent or nonadjacent), the number of layers is determined by the chronologically

last selected zone in the Boundary Zones selection list.

Important

– If you specify different number of layers to be grown on adjacent zones, the same

number of layers (generally the smaller number of layers) will be grown on both the

zones (see Figure . : Different Growth Parameters on Adjacent Zones (p. )).

– If you specify different number of layers on multiple (nonadjacent) zones and use the

Prisms dialog box to generate the prism layers, the same number of layers will be grown

on the respective zones.The number of layers is determined by the chronologically last

selected zone in the Boundary Zones selection list.

Auto Mesh dialog box to generate the prism layers, the prism layers will be grown

separately from each zone:

Figure . : Different Growth Parameters on Nonadjacent Zones—Using the

Auto Mesh Option

Two-sided walls may be present in some models. To grow prisms on both sides of a two-sided wall

(for example, growing prisms on dangling walls), do the following:

.

Select the two-sided wall on which you want to grow prisms from the Boundary Zones selection list.

.

.

.

Specify the prism growth parameters as required.

.

Enable Grow on Two Sided Wall in the Growth tab of the Prisms dialog box.

.

Click Create. Figure . : Prism Growth on a Dangling Wall (p. ) shows an example of prisms grown

on a dangling wall.

Figure . : Prism Growth on a Dangling Wall

Some models may contain regions where the normals considered while growing prisms may be invalid.

The normal at a particular node may be nearly tangential to the surrounding faces in the model and

as a result, the prism generation may fail. For such cases, you can choose to ignore regions of the

model where invalid normals exist, during prism generation. Prism layers will be grown from the re-

maining regions according to the specified parameters.

Figure . : Ignoring Invalid Normals (p. ) shows a portion of the model where the normal at the

highlighted node will be nearly tangential to some of the surrounding faces. You can see that the

region around this node has been ignored while creating prisms.

Figure . : Ignoring Invalid Normals

You can ignore regions based on normals while creating prisms as follows:

.

Specify the prism growth parameters.

.

Select the Boundary Zone containing the invalid normal and click the Growth Options... button to

open the Prisms Growth Options dialog box.

a.

Enable Ignore Invalid Normals in the General Options group box.

b.

Click Apply and close the Prism Growth Options dialog box.

.

Grow prisms as required.

b.

.

If the zones on which you want to grow prisms are very close to each other, the prism layers from

zones may intersect or collide with each other. This results in bad quality of prism layers.

For example, in Figure . : Collision of Prism Layers (p. ), the prism layers grown from proximal

surfaces intersect each other. The Allow Shrinkage option allows you to avoid the intersection of

prism layers by adjusting the height of the prism layers in closely placed zones. Figure . : Prism

Layers Shrunk to Avoid Collision (p. ) shows the use of this option to avoid intersection of the

prism layers by adjusting the prism layer height.

Figure . : Collision of Prism Layers

Figure . : Prism Layers Shrunk to Avoid Collision

A value of n for Gap Factor implies that a gap equal to n times the maximum base edge length at

the node in question will be maintained. Hence, a value of  implies that the gap maintained is equal

to the maximum base edge length at the node considered.

Important

Offset heights are scaled only in the regions where the intersection of prism layers takes

place. For the remaining regions, the prisms are created according to the specified para-

meters.

You can also ignore prisms in regions of close proximity during prism generation. The area of proximity

will be determined based on the shrink factor specified. Prism layers will be grown from the remaining

regions according to the specified parameters.

Figure . : Ignoring Areas of Proximity (p. ) shows a portion of the model where the region of

proximity in a sharp corner has been ignored while creating prisms.

Figure . : Ignoring Areas of Proximity

For automatic adjustment of intersecting/colliding prism layers while growing prisms, do the following:

.

.

Click Growth Options... in the Growth tab to open the Prisms Growth Options dialog box.

.

Enable the appropriate options in the General Options group box.

.

Specify the parameters required for the proximity calculation and controlling the prism layer height.

a.

Enable Allow Shrinkage to allow shrinkage of prism layers in areas of proximity.This option is

b.

Enable Keep First Layer Offsets, if required.

This option allows you to keep the original first offset height and scale the offset heights

for the remaining layers in case of intersecting prism layers.

c.

Specify an appropriate value for Gap Factor.

d.

Enable Allow Ignore to ignore the prism growth parameters in areas of proximity.

e.

Enter an appropriate value for Max Aspect Ratio or Max Shrink Factor as required.

f.

.

Click Create in the Prisms dialog box.

You can generate fewer prism layers and then split them as part of the prism generation process to

generate the total number of prism layers required. This option is faster than generating the same

total number of prism layers.

You can specify the number of divisions per prism layer as follows:

.

.

.

.

Click Growth Options... to open the Prisms Growth Options dialog box.

.

Enable Split in the Split Options group box.

.

Specify the Divisions Per Layer.

.

In some cases, it may be important for the prismatic mesh to be orthogonal near the original

boundary. For such cases, there are two ways to preserve orthogonality:

Decrease the value specified for the Max. Angle Change in the Direction tab of the Prisms dialog box

to a lower value to limit the change in normal direction in each prism layer.

This parameter is set to  degrees by default. This means the normal direction at a node can

change up to  degrees during normal, edge, and node smoothing. For example, if you reduce

this parameter to  degrees, the change in normal direction will be more gradual, and the mesh

near the original boundary will be nearly orthogonal.

Specify an explicit number for Orthogonal Layers in the Direction tab of the Prisms dialog box.

When you specify orthogonal layers, you should decrease the Max Angle Change to approximately

degrees. This will prevent sudden sharp changes in normal direction at the first non-orthogonal

layer.

For a non-orthogonal layer, edge swapping, normal, edge, or node smoothing will be performed

so that the layer is orthogonal to the original boundary. For example, if you specify  orthogonal

layers, no smoothing will be performed on the first  layers, resulting in direction vectors that are

normal to the original surface mesh faces. Full smoothing is used on the sixth and subsequent

layers.

layers.

Important

If you are preserving orthogonality near the original boundary, make sure that the prism

layers do not grow too quickly. Use small layer heights, relative to the sizes of the faces

on the original boundary. If prism layers grow quickly, the nearly-orthogonal direction

vectors are likely to cross at sharp concave corners, causing the prism generation to fail.

The prism layer generation will be stopped at this point. See Normal Smoothing (p. ).

Preserving orthogonality can affect skewness and lead to left-handed faces and/or negative volumes.

See Negative Volumes/Left-Handed Faces/High Skewness (p. ) for details.

The offset distance for a given node is the distance between adjacent layers at that node. This distance

is based on the prism layer height computed from the specified prism growth parameters. The new

node for a prism layer is placed at this distance along the direction vector.

There are four methods available for determining the offset distances:

Uniform Offset Distance Method: In this method, every new node (child) is initially the same distance

away from its parent node (that is, the corresponding node on the previous layer, from which the direction

Figure . : Uniform Offset Distance Method

Uniform distances are fine for planar surface meshes, but they result in crevices at sharp corners,

for example, the  degree corner in Figure . : Uniform Offset Distance Method (p. ). The dir-

ection vector at the corner node will be at an angle of  degrees, while the vectors at the adjacent

nodes will be slightly more orthogonal to their faces. For uniform distances, this places the nodes

for the first layer as shown in Figure . : Uniform Offset Distance Method (p. ).

The dashed line connecting the new nodes begins to pinch inward at the corner. The distances

between parent and child nodes are still all the same, but the angles of the direction vectors introduce

this pinching effect. Without some sort of correction such crevices can eventually collapse.

Minimum Height Offset Distance Method: In this method, child nodes are guaranteed to be at least as

far from their parent nodes as the distance computed for the current layer from the growth inputs.The

mesher will also try to retain the shape of the original boundary.

Figure . : Minimum-Height Offset Distance Method

For a perfect  degree corner, this results in a perfect  degree corner for the next layer (see Fig-

ure . : Minimum-Height Offset Distance Method (p. )). Thus, in this method the shape is better

preserved if no additional smoothing is applied.

The minimum height method have some limitations. If the angle of the direction vector at the corner

is not  degrees (that is, if it does not exactly bisect the angle between the faces), the minimum-

height method can increase skewness.

Aspect Ratio Method:This method allows you to control the aspect ratio of the prism cells that are extruded

from the base boundary zone.The aspect ratio is defined as the ratio of the prism base length to the prism

layer height.The various growth methods (constant, linear, geometric, and exponential) can be used to

specify the aspect ratio of the first layer.

When a non-constant growth method is used, the aspect ratio for subsequent layers will change

accordingly. The heights of the prism cells will vary according to the local face sizes in the surface

mesh, providing a convenient way to automatically vary prism heights across a zone.

Last Ratio Method:This method also allows you to control the aspect ratio of the prism cells that are ex-

truded from the base boundary zone.You can specify First Height for the first prism layer. If you select

this method, the various growth methods will not be accessible.The last aspect ratio method is explained

in Figure . : Last Ratio Method (p. ).

Figure . : Last Ratio Method

Local base mesh size is used to find out the offset height for the last layer. For example, if you specify

as the Last Percent value the offset height of the last layer will be . times the local base mesh

size. Local growth rate is used to calculate the other intermediate offset heights exponentially.

Note

Once calculated, the actual last last layer offset height is not adjusted in cases of

concave or convex base, or non-orthogonal layers.

Offset Smoothing

The purpose of offset smoothing is to eliminate spikes and dips in the new surface layer. Smoothing

is applied iteratively. Figure . : Effect of Offset Smoothing (p. ) shows how the nodes are moved

during offset smoothing.

Figure . : Effect of Offset Smoothing

As each layer of prisms is built, the mesher needs to know the direction in which to build. There are

two methods available for determining the direction vectors:

Extrusion Method: For creating straight-sided prism regions without any curvature, you can specify a

uniform direction vector for all prism layers. Select Uniform in the Method list in the Direction tab of the

Prisms dialog box.

Figure . : Uniform Direction Vector for a Straight-Sided Prism Region

Specify the uniform direction vector or click Compute in the Vector group box. This constant vector

will be used for all prism layers, instead of computing a new direction for each layer (see Fig-

ure . : Uniform Direction Vector for a Straight-Sided Prism Region (p. )).

Note

The Grow On Two Sided Wall option cannot be used when the Uniform method is se-

lected.

Normal Method: For regions with curvature, the appropriate normal direction vector at each node will be

determined because it may be different for each node and each layer. See Figure . : Normal Direction

Vectors for a Curved Prism Region (p. ). Select Normal in the Method group box in the Direct tab of

Figure . : Normal Direction Vectors for a Curved Prism Region

Normal Smoothing

The normal direction vectors obtained using the methods described in Direction Vectors (p. ) are

smoothed so that there is a gradual change in direction from one node to the next. This will reduce

the chance of direction vector intersection, which causes the prism generation to fail. This step is not

necessary when a uniform direction vector is used because there is no change in direction from one

node to the next.

Figure . : Normal Direction Vectors Before Smoothing (p. ) shows normal direction vectors in

the vicinity of a sharp ( degree) corner.

Figure . : Normal Direction Vectors Before Smoothing

The direction vector is at an angle of  degree at the corner, while elsewhere it is  or  degrees.

These direction vectors will intersect and prisms cannot be generated. Figure . : Normal Direction

Vectors After Smoothing (p. ) shows the normal direction vectors near the corner after they have

been smoothed. After smoothing, the normal direction changes more gradually from node to node.

Figure . : Normal Direction Vectors After Smoothing

It is possible to create very thin prism layers using the direction vectors shown in Figure . : Normal

Direction Vectors Before Smoothing (p. ), as long as the last layer lies below the point where the

vectors cross.

For each zone adjacent to the zones from which you grow prisms, the angle between the prism growth

direction and the adjacent zone will be checked. Depending on the size of this angle, the mesher will

decide whether to use the adjacent zone for the prism sides, or create a new zone.

Using Adjacent Quadrilateral Face Zones

An adjacent zone with quadrilateral faces will be used without modification as the prism-side boundary

if it satisfies the following requirements:

It must share nodes with the boundary zone from which you are building the prisms that is, there must be

no free nodes (see Free and Isolated Nodes (p. )) where the zones touch.

The angle between the adjacent zone and the prism growth direction must be less than the specified

threshold, Max. Adjacent Zone Angle (in the Project tab of the Prisms dialog box).The default threshold

value is  degrees.

For example, if you are growing prisms from the bottom surface in Figure . : Effect of Adjacent

Zone Angle (p. ) using the default maximum adjacent zone angle of  degrees, the zone on the

left will be excluded, but the zone on the right will be used as it is. A new zone will be created for the

left sides of the prisms.

Figure . : Effect of Adjacent Zone Angle

To fill in the gap on the left side of Figure . : Effect of Adjacent Zone Angle (p. ), create pyramids

using the prism side faces, create a domain, and generate tetrahedral cells.

Projecting to Adjacent Triangular Face Zones

If an adjacent zone has triangular faces, two additional steps will be performed to incorporate the

zone into the prism layers: projection  and retriangulation. The mesher will project the outer nodes of

the prisms onto the triangular faces of the adjacent zone, provided it satisfies the following requirements:

It must share nodes with the boundary zone from which you are building the prisms.That is, there

must be no free nodes (see Free and Isolated Nodes (p. )) where the zones touch.

threshold, Max. Adjacent Zone Angle (in the Project tab of the Prisms dialog box).The default

threshold value is  degrees.

In Figure . : Effect of Adjacent Zone Angle (p. ), the zone on the right will be projected to and

retriangulated, while the zone on the left will be excluded.

Retriangulation

As shown in Figure . : Prism Shapes (p. ), the sides of the prism will always be quadrilateral faces,

regardless of the type of face from which the prism is built (triangular or quadrilateral). If the prism-

side nodes are projected to an adjacent triangular boundary face zone:

.

The prism-side faces on the shared boundary will be overlaid on the triangular faces of the existing

.

The triangular boundary zone will be retriangulated so that the triangular portion of the zone ends at

the border of the portion now filled with quadrilateral faces.This is done to obtain a conformal mesh

where all the nodes match up at face edges.

.

The triangles that were overlapping the quadrilateral prism-side faces will be deleted.

Figure . : Symmetry Zone and Car Wall Before Prism Generation (p. ) shows the initial boundary

mesh for a car and the symmetry boundary beside it. If the prisms are generated from the car body

without retriangulation of the triangular symmetry boundary, the resulting boundary mesh will be as

shown in Figure . : Symmetry Zone and Car Wall After Prism Generation Without Retriangula-

tion (p. ). With retriangulation, the boundary mesh will appear as in Figure . : Symmetry Zone

and Car Wall After Prism Generation and Retriangulation (p. ).

Figure . : Symmetry Zone and Car Wall Before Prism Generation

Figure . : Symmetry Zone and Car Wall After Prism Generation Without Retriangulation

Figure . : Symmetry Zone and Car Wall After Prism Generation and Retriangulation

Important

Though it is possible to disable retriangulation (by disabling the Retriangulate Adjacent

Zones option in the Project tab of the Prisms dialog box), it is not always recommended.

Expert users experimenting with different settings may temporarily disable retriangulation.

You can choose to improve prism mesh quality by swapping or smoothing edges, and smoothing

nodes. These options are switched off by default.

.... Edge Swapping and Smoothing

.... Node Smoothing

You can choose to improve prism mesh quality by swapping or smoothing edges. After the new cap

faces are created for the new layer, the skewness is compared with the specified skewness threshold

(Skewness in the Swapping and Smoothing group box in the Improve tab of the Prisms dialog

box). If the skewness of a face is too high, the following improvement procedure is carried out:

.

Swap the longest edges of highly skewed faces.

When edge swapping occurs on a cap face, swapping propagates downward. Swapping must

be performed on the corresponding faces on all prism layers, including the face on the original

boundary mesh, so that the grid lines within the prism layers do not cross.

Important

Swapping is not performed if it will significantly alter the geometry defined by the

original boundary mesh.

.

Important

.

If swapping is not performed, the skewness will be improved by smoothing the nodes of the skewed

faces using one of the following operations.

If the sharpest angle at the node (that is, the most acute angle between adjacent faces that use the

node) is nearly  degrees, smoothing will be performed (as described in Node Smoothing (p. ))

to move the nodes.

If the sharpest angle is far from  degrees, the smoothing will be limited so that the nodes are only

allowed to move along the face’s longest edge.This method will prevent the collapse of sharp corners

in the mesh.

Note

Smoothing does not propagate downward, it is performed only on the skewed cap

faces themselves.

Important

This edge swapping/smoothing procedure is not performed on quadrilateral cap faces.

If the edge swapping and smoothing are not sufficient to reduce the skewness of some faces, you

can include an additional smoothing operation. In this method, if any of the faces surrounding a new

node have a skewness greater than the specified threshold, the node is smoothed.

Instead of moving only the node, this method will also move the surrounding nodes to make space

for the node to move.

Figure . : Node Smoothing in Rings

The surrounding nodes are grouped and smoothed in rings (see Figure . : Node Smoothing in

Rings (p. )). The nodes on the outermost ring are smoothed first, and so on, until the target node

(on ring zero) is finally smoothed.

This type of smoothing is helpful in concave areas where the advancing layers continually decrease

the available surface area, causing squashing of triangular faces. By smoothing outer rings of nodes

first, more space is provided for the nodes that need to be moved in order to reduce the skewness.

Thus, this method performs regional smoothing around faces of high skewness. The node smoothing

procedure can be performed on both tri and quad faces.

You can improve prism cell quality in a postprocessing step after all the required prism layers are

created. The following options are available:

.... Improving the Prism Cell Quality

.... Removing Poor Quality Cells

.... Improving Warp

The Prism Improve dialog box contains options that allow you to improve the prism cell quality

based on the quality measure selected. The quality measures available are ICEM CFD quality, orthoskew,

skewness, or squish. The following options are available:

The Smooth option allows optimization based smoothing of prism cells. Poor quality cells can be identified

based on the quality measure selected.The nodes of cells with quality worse than the specified Max Cell

Quality value will be moved to improve quality.The cell aspect ratio will also be maintained based on

the value specified for max-aspect-ratio.

The Improve option collects and smooths cells in layers around poor quality cells. Poor quality cells can

be identified based on the quality measure selected. Cells with quality worse than the specified Max Cell

Quality value will be identified, and the nodes of the cells surrounding the poor quality cells will be moved

to improve quality.The cell aspect ratio will also be maintained based on the value specified for max-

aspect-ratio.

The Smooth and Improve option uses a combination of node movement and optimized smoothing to

improve the quality.This option is a combination of the Smooth and Improve options.The cell aspect

ratio will also be maintained based on the value specified for max-aspect-ratio.

When the Smooth and Improve option is enabled in the Post Operations group box in the Improve

tab of the Prisms dialog box, the prism cells will be improved based on the options selected in the

Prism Improve dialog box, after the required prism layers are created.

You can alternatively use the options in the Prism Improve dialog box to improve the prism cell

quality in a postprocessing step after the mesh is created.

Mesh → Tools → Prism → Improve

In cases where the prism mesh is created separately (without using the Merge Cell Zones option in

the Auto Mesh tool) and the prism-cap zone exists, you can use additional options to remove layers

of poor quality cells in regions of poor quality and sharp corners.

The Prism Post Ignore dialog box contains options that allow you to remove poor quality prism cells

based on quality, intersection, interior warp, and feature edges.You can specify the number of cell rings

to be removed around the marked cells. Cells will be marked for removal in regions of sharp corners based

on the Ignore Options selected and then extended based on the number of cell rings specified. Additional

cells will be marked for removal in regions of high aspect ratio and feature angle (if selected in the Expand

Ignore Options group box) around the exposed prism side.

The Feature Edges tab contains options for manipulating feature edges to be used for the post-

ignore operation. You can extract edge zones from the prism base zones when the prism cap zone

is selected in the Boundary Zones list. The edge zones are extracted based on the Feature Angle

specified. Other operations like merging or separating the edge zones are also available.

The boundary will be smoothed at feature corners after the prism cells have been removed. The

prism-side faces exposed by the removal of the prism cells will be collected in a zone named

prism-side-#, while for a zone wall-#, the faces corresponding to the ignored prism cells will

be collected in a zone named wall-#:ignore. You can also optionally smooth the prism side

nodes from the base node to the cap node to create better triangles for the non-conformal interface.

When the Ignore option is enabled in the Post Operations group box on the Improve tab of the

Prisms dialog box, the prism cells will be removed based on the options selected in the Prism

Post Ignore dialog box, after the required prism layers are created.

Note

The Feature Edge option, under Ignore Options in the Prism Post Ignore dialog

box, requires a prism-cap zone to be present so it cannot be used as a Post Oper-

ation control during prism generation.

You can alternatively use the options in the Prism Post Ignore dialog box to remove layers of poor

quality cells in a postprocessing step after the mesh is created.

Mesh → Tools → Prism → Post Ignore

The Prism Tet Improve Cavity dialog box contains options for creating a cavity in regions where the

prism quality is adequate, but the quality of adjacent tetrahedra is poor.The cavity is created based on

the tetrahedral cell zone, the quality measure and the corresponding threshold value specified. Additional

cells will be removed based on the number of expand cell rings specified.You can create a cavity comprising

only tetrahedral cells or optionally include prism cells when the cavity is created.When prism cells are

also included in the cavity, you can specify whether the non-conformal interface is to be created.

Mesh → Tools → Prism → Tet Improve Cavity

Improving warp in prisms is a postprocessing step which is carried out after all the required prism

layers are created. The face warp in the generated prism faces is improved by moving the nodes of

the face to make it planar.

When the Improve Warp option is enabled in the Post Operations group box in the Improve tab

of the Prisms dialog box, the prism layers having faces with warp ≥ . are identified. The nodes on

the identified faces are moved and the new location of the node is updated only when:

. The overall maximum warp of the faces connected to the node has decreased.

. The overall maximum skewness of the cells connected to the node has decreased or remained the same.

This is useful in regions having complex sharp corners, where the nodes of a prism cell may have

drastic normal change.

.. Prism Meshing Options for Scoped Prisms

Scoped prism controls allow you to apply prism layer parameters to specific regions of the mesh object.

Accessible through the Auto Mesh volume-meshing tool, the scoped prism process first creates

boundary layers based on the defined controls, and then proceeds to generating the tet/hexcore mesh.

Important

Volumetric regions need to be computed prior to object based volume meshing.The computing

of regions includes topology checks, re-orienting of normals, and baffle identification and

The direction of prism growth does not need to be set up separately.The prism layers are always

grown into the regions selected; normals are re-oriented accordingly when the regions are

computed.

The scoped prisms method does not use any of the settings made in the Prisms dialog box or

using the commands in the /mesh/prism menu.

To set up scoped prism controls, select scoped from the Grow Prisms drop-down list in the Auto Mesh

dialog box and click Set... to open the Scoped Prisms dialog box.

You use the Scope To drop down list to select fluid or solid regions.

You can select fluid-regions, solid-regions, or named-regions. If named-regions is selected, you

can enter the region name (wildcards supported) in the Volume Scope field or click the Browse

button (

) and select the regions in the Volume Scope dialog box.

Within the selected regions, you use the Grow On drop-down list to select the boundary type on which to

grow prism layers.

You can use all-zones for unrestricted boundary type. Alternatively, use only-walls to scope prism

growth by wall boundary type. To scope prisms by boundary name, use selected-labels, selected-

face-zones, or solid-fluid-interface and enter the name or pattern in the Boundary Scope field, or

click the Browse button (

) to use the Boundary Scope dialog box.

If interior baffles exist, the Grow on both sides of baffles option will be available. You can choose

to grow prisms on both sides (default) or on a single side. In case of single side, use the Color by

Normal option (hot-key combination Ctrl+Shift+C and Ctrl+N) to see on what side (gray) the prisms

will grow.

You use the Offset Method drop down list to select from uniform, aspect-ratio, or last-ratio as the prism

offset method.The geometric growth method is used; you can specify the growth rate as appropriate.

A meaningful Name is recommended.

Important

Fluent Meshing supports multiple scoped prism controls, however only one scoped prism

control can be applied to a face zone in a given region.

Prism Meshing Options for Scoped Prisms

In Figure . : Use of Multiple Scoped Prism Controls (p. ), prism layers are grown on

adjacent zones within the fluid region, but with multiple scoped controls defined. The prism

layers are stair stepped to obtain a gradual transition between the layers. Also, solid-fluid-

interface is selected from the Grow On drop-down list, to enable growth of different number

of layers in the solid and fluid regions.

Figure . : Use of Multiple Scoped Prism Controls

Note

The scoped prism controls can be read from a previously saved file (*.pzmcontrol) or can be

written to a file for further use.

The command /mesh/scoped-prisms/set-no-imprint-zones enables you to specify

boundary zones which should not be imprinted during the prism generation.

Proximity Handling

Once the initial prism layers are generated, the prism mesh is improved by a combination of optimization-

based smoothing and node movement to smooth the prism cell layers. The scoped prisms approach

includes two steps of collision avoidance—layer compression and stair stepping. Use the Growth Options

button to setup controls to avoid collision of prism layers in proximal regions.

Enable Keep First Layer Offsets to preserve the first offset height as other layers are modified to prevent

collisions.

In regions of close proximity the prism layers are first compressed to resolve gaps and sharp corners,

based on the Gap Factor and Max Aspect Ratio specified.

After this, cells are identified for stair stepping — a post prism meshing process carried out to avoid

prism layer collision and maintain mesh quality. In areas where it is not possible to meet the quality

limit specified by the Stair Stepping Threshold, or where intersections are detected, the higher prism

layers will be removed and filled with pyramids and tetrahedra as transition elements between the re-

maining layers and the volume fill. A list of locations where the prism layers were stair stepped is printed

in the console. For prism meshing, it is recommended to use ICEM CFD Quality as the quality method

since it is more stringent than the Skewness metric.

If the final mesh quality is not acceptable, you can use the Auto Node Move tool with ICEM CFD

quality measure to improve the mesh.

Figure . : Stair Stepped Prism Layers in Sharp Corner (p. ) shows an example of a sharp corner

where the prism layers have been stair stepped.

Figure . : Stair Stepped Prism Layers in Sharp Corner

.. Prism Meshing Problems

This section discusses a number of common problems that you may encounter when generating pris-

matic meshes. An appropriate solution is also recommended for each problem. If the prism generation

fails or is unsatisfactory, you may read in the mesh you saved before starting the prism generation (in

step  of Procedure for Creating Zone-based Prisms (p. )) and repeat the process, incorporating the

appropriate corrections.

The most common prism meshing problems are:

Orientation

Retriangulation failures

Too many or too few nodes, or unknown face combinations

Negative volumes, left-handed faces, or high skewness

Prism Meshing Problems

Growing too far

Large jumps in prism height at the edges of layers

If the faces of the boundary zone from which you are building prisms are not all oriented in the same

direction, you will be alerted that the faces have been reoriented, and the prism generation process

will proceed.

Retriangulation Failures

If nodes, where adjacent zones meet the zones (from which prisms are growing) are duplicated, the

mesher will be unaware that the zones are connected. It will ignore such zones when considering nodes

for projection, and hence retriangulation is likely to fail.

Solution: To verify this problem check the messages printed before the first prism layer. It should

contain a list of all the zones connected to the zones from which you are growing the prisms.

.

Make sure there are no free nodes in the surface mesh before growing any prisms.

.

Use the Count Free Nodes button in the Merge Boundary Nodes dialog box to check for free nodes.

.

Enable the Free option in the Faces section of the Display Grid dialog box to see where the free nodes

are located.

Too Many/Few Nodes or Unknown Face Combinations

If you receive the following type of messages, then you are most likely growing prisms into existing

cells.

Warning: wedge cell c887 has too many nodes

Warning: wedge cell c1928 has too few nodes

Warning: base_mask =  (0x7), unknown face combinations

Either you have already grown prisms from the selected zones, or you are growing them in the wrong

direction into cells on the other sides of the selected zones. In the latter case, reorient the normals and

growing the layers. See step  in Procedure for Creating Zone-based Prisms (p. ).

Negative Volumes/Left-Handed Faces/High Skewness

The prism layer creation process will automatically stop if negative cell volumes,  left-handed faces, or

high skewness are detected.

Left-handed faces are faces that have collapsed into their cells. You can view them by enabling the Left

Handed option in the Faces section of the Display Grid dialog box. Very high skewness occurs when

the value of skewness is greater than the specified Max. Allowable Skewness in the Improve section

of the Prisms dialog box). These problems can occur where prism layer fronts are advancing too quickly

in areas of high curvature.

For example, the first layer height may be greater than the minimum edge length of your original surface

mesh. You should compare the First Height with the results of clicking the Edge Size Limits button

in the Growth section of the Prisms dialog box. The First Height should usually be smaller than the

minimum edge size.

Solution: If the First Height is reasonable but you are unable to successfully generate your requested

Total Height, try one of the following solutions:

Reduce the First Height or the parameter used for the growth Method (that is, Slope, Rate, or Exponent),

and increase the Number of Layers. Extra layers allow smoothing to compensate better for sharp edges

and corners.

If you have specified a nonzero value for Orthogonal Layers (in the Direct section of the Prisms dialog

box), change it to zero. Increasing orthogonality can reduce robustness.

If you have reduced the Max. Angle Change (in the Direct section of the Prisms dialog box) from its default

of  degrees to improve orthogonality, reset it to .

If you have disabled edge swapping or normal, offset, or edge smoothing, turn them back on.

If you are using the minimum-height offset method (enabled with the mesh/controls/prism/offset-

methodtext command), switch back to the uniform method.

Lower the Skewness for Swapping and Smoothing in the Improve section of the Prisms dialog box.

Increase the number of Layers in the Improve section of the Prisms dialog box if it is smaller than the

number of layers being grown.

Enable Smooth Nodes in the Improve section of the Prisms dialog box.You can also increase the number

of smoothing rings, using the command:

/mesh/controls/prism/node-smooth-rings

If you are growing simultaneously from multiple zones, use zone-specific growth controls. Use smaller initial

heights and/or growth rates for zones that are having problems.

Growing Too Far

The problem here is growing too many layers. Ideally, to provide for a smooth transition to the nearly-

equilateral tetrahedra, the volume of the tetrahedra should be the local growth rate times the volume

of the last layer prism cells.

Solution: To ensure this does not happen, verify that the prism parameters satisfy the above condition.

Large Jumps in Prism Height

If the prisms use quadrilateral faces of adjacent zones, and the node spacings on these faces are very

different from the layer heights, the prism heights jump at the outer edges.

Solution: To fix this problem, replace the adjacent quadrilateral face zones with triangular face zones,

using the /boundary/remesh/triangulate text command. When you reattempt the prism gen-

eration, the zone will be projected to and retriangulated.

Because the outer nodes of the prisms are projected to the adjacent boundary zone, and the original

nodes on that portion of the zone are discarded, the different node spacing on the adjacent zone will

not affect the prism heights at the outer edges.

Chapter : Generating Tetrahedral Meshes

This chapter describes how to create the tetrahedral mesh in the domain. It also describes some of the

common problems faced during tetrahedral meshing.

You can use one of the following techniques to generate tetrahedral meshes:

Automatic mesh generation (see Automatically Creating a Tetrahedral Mesh (p. ))

Manual mesh generation (see Manually Creating a Tetrahedral Mesh (p. ))

A combination of manual and automatic commands (see Initializing the Tetrahedral Mesh (p. ), Refining

the Tetrahedral Mesh (p. ))

If the cells (for example, prisms or pyramids) have already been created in some portion of the compu-

tational domain, you need to create a domain encompassing the region to be meshed with tetrahedral

cells before starting with the tetrahedral mesh generation. See Using Domains to Group and Mesh

Boundary Faces (p. ) for details. In such cases, all automatic and/or manual meshing actions will apply

only to the active domain.

Alternatively, instead of creating a new domain, you can specify the cell zones to be preserved while

generating the tetrahedral mesh, before proceeding with the mesh generation. You can use the command

/mesh/tet/preserve-cell-zone to specify the cell zones to be preserved.

.. Automatically Creating a Tetrahedral Mesh

The Mesh → Auto Mesh feature contains commands that encapsulate the recommended volume mesh

generation strategy. The starting point for this procedure is a valid surface mesh.

... Automatic Meshing Procedure for Tetrahedral Meshes

... Using the Auto Mesh Tool

... Automatic Meshing of Multiple Cell Zones

... Automatic Meshing for Hybrid Meshes

... Further Mesh Improvements

The automatic tetrahedral mesh generation process is divided into two fundamental tasks: initialization

and refinement.

The automatic initialization procedure includes the following steps:

. Merging free nodes.

. Deleting unused nodes.

. Improving the surface mesh.

. Initializing the mesh.

. Generating and separating cell regions.

Important

If the mesh fails to initialize, typically this indicates a problem with the surface mesh.

In some rare cases, the sliver size (which is automatically computed) may need to be

changed. This may happen for domains in which the minimum boundary face size is

very small as compared to the domain extent. When changing the sliver size, the rule

of thumb is that the specified value should be of the order 1e- times the minimum

face area.

The automatic refinement procedure includes the following steps:

. Sorting the boundary faces by size.

. Refining the boundary cells.

. Reverse sorting cells by skewness.

. Refining the active cell zones.

. Swapping cells based on skewness.

. Smoothing the mesh.

. Removing boundary slivers.

You can select either the advancing front refinement, or the skewness-based refinement of the tetra-

hedral mesh. The refinement procedure is repeated a number of times.

You can control the number of repetitions for skewness-based refinement by setting the Number of

Levels in the Tet Refine Controls dialog box. For each subsequent level of refinement, the cell

skewness thresholds are lowered. Additional refinement levels increase the mesh resolution (and the

number of cells) and decrease the average cell skewness.

Each refinement level actually consists of two sweeps through the refinement procedure:

One sweep at the appropriate skewness threshold for that particular level of refinement.

Another sweep with a high skewness threshold and a relaxed Min Boundary Closeness set in the Tet

Refine Controls dialog box.

This sweep attempts to reduce highly skewed cells in confined regions of the geometry.

Boundary slivers will be removed after the refinement sweeps are complete if the Remove Slivers

option is enabled in the Refinement tab of the Tet dialog box.

In some rare cases, it may happen that the first sweep of the first refinement level will never finish

because more skewed cells are formed due to refinement, which will be further refined to create more

skewed cells, and so on. Such a problem may occur when there is a problem with the boundary mesh,

Generating Tetrahedral Meshes

such as rapid mesh transition in small gaps, and so on. You can avoid this problem by using the incre-

mental improvement option for the refinement parameters or by increasing the Min Node Closeness

value in the Tet Refine Controls dialog box.

You can select the fast transition option for the refinement parameters in order to generate a mesh

with a smaller number of cells. When this option is selected, appropriate refinement parameters will

be used to generate fewer cells during meshing. The rate of change of the cell size is increased in order

to reduce the number of cells generated. Alternatively, you can specify an appropriate cell sizing option

with a sufficiently large value for the growth rate.

Important

Important

Various steps in the automatic meshing process can be added or eliminated using the Tet

dialog box. In addition, most aspects of the automatic meshing process can be changed

dynamically through the Scheme interface. Contact your support engineer for details.

You can use the Mesh → Auto Mesh tool to automatically:

Generate a tetrahedral volume mesh starting from a boundary mesh.

Generate a tetrahedral volume mesh in an unmeshed domain of a mesh that contains other cell shapes.

The Auto Mesh tool enables you to generate the tetrahedral volume mesh automatically. When you

select Tet in the Volume Fill list and click Mesh in the Auto Mesh dialog box:

If the volume mesh does not exist, all the steps listed in Automatic Meshing Procedure for Tetrahedral

Meshes (p. ) will be performed.

If a volume mesh already exists, a Question dialog box will appear, asking if you want to clear the existing

mesh. If you click Yes, the volume mesh will be cleared and the active steps in the automatic mesh gener-

ation process will be performed. If you click No, the operation will be canceled.

Important

You can use the command /mesh/tet/preserve-cell-zone to specify the cell

zones to be preserved during mesh generation and click Mesh to proceed with the

automatic mesh generation.

The Auto Mesh tool enables you to mesh multiple cell zones automatically. This is useful when the

mesh has multiple cell zones (for example, the problem requires a fluid zone and one or more solid

zones). You can refine the mesh using refinement parameters specific to individual zones, if required.

The procedure for meshing multiple cell zones includes the following steps:

. Initialize the mesh.

. Activate the appropriate zones using the Manage Cell Zones dialog box.

Automatically Creating a Tetrahedral Mesh

. Set the zone-specific refinement parameters and refine the active zones.

If you want to mesh all the zones included in the mesh with the same refinement parameters,

modify the Non-Fluid Type in the Tet dialog box.

Important

By default, the Non-Fluid Type is set to dead as the mesh is assumed to consist of a

single fluid region and one or more dead regions. The active zone is considered to be

the fluid zone and only this fluid zone will be considered for refinement during the

automatic meshing process.

When the Non-Fluid Type is set to a type other than dead (for example, solid), all the

zones will be active after the initialization is complete. Hence, all the zones will be con-

sidered for refinement. If required, you can change the zone type using the Manage

Cell Zones dialog box.

Select the appropriate type from the Non-Fluid Type drop-down list in the Tet Zones group box

in the Tet dialog box before initializing the mesh.

Note

For zone-based meshing, if any cell zone has at least one boundary zone type as inlet,

it will automatically be set to fluid type. For object based meshing, volume region type

is used to determine the cell zone type.

The Auto Mesh tool can also create prisms and pyramids automatically, allowing automatic generation

of hybrid meshes.

If a mix of surface mesh types (quadrilateral and triangular) is present in the domain, pyramid cell zones

will be created on the quadrilateral boundary faces before meshing the tetrahedral domain.

If prism growth parameters have been attached to a boundary zone (using the Prisms dialog box), the

prism layers will be automatically extruded before meshing the tetrahedral domain.

When pyramids or prisms are generated using the automatic mesh generation feature, the interme-

diate boundary zones will be merged automatically after the tetrahedral mesh generation is complete.

This enhancement avoids the creation of additional boundary zones such as prism-side and pyramid-

cap (see Zones Created During Prism Generation (p. ) and Zones Created During Pyramid Gener-

ation (p. )).

You can transition from quad to tri faces using the Non Conformals option.This option is useful when you

want to avoid pyramids on quad faces when growing prisms from a boundary. For mixed surface mesh

types (quadrilateral and triangular), you can select Non Conformal in the Quad Tet Transition list in the

Auto Mesh dialog box.The surfaces containing quad faces will be copied and triangulated, keeping the

original faces intact.The free nodes of the triangulated surface will then be merged with the nodes of the

original surface mesh and both the surfaces will be converted to interface type.

Examine the following after completing the automatic mesh generation process:

The mesh size with the Report Mesh Size dialog box (see also Determining Mesh Statistics (p. )).

The prism layer cell quality distribution (see Determining Boundary Cell Quality (p. )), if appropriate.

The tet cell quality reports (see also Determining Volume Mesh Quality (p. )).

It is typically possible to reduce the maximum skewness to the range .–.. Skewness values higher

than . are typically obtained due to constraints imposed by the surface meshes. If you still have

highly skewed cells apply additional swapping and smoothing to improve the quality (see Smoothing

Nodes (p. ) and Swapping (p. )). To increase the density of the mesh locally, use refinement regions

(see Using Local Refinement Regions (p. )).

Warning

Do not over-refine the mesh. The volume mesh produced should be of sufficient density

to resolve the shape of the geometry. The mesh can be improved more effectively using

the solution-adaptive mesh capability provided in the solution mode in Fluent.

.. Manually Creating a Tetrahedral Mesh

In addition to the Auto Mesh tool, you can control the tetrahedral mesh generation process by modi-

fying parameters at each step. The basic operations are described here, and the methods for modifying

the associated parameters are described in Initializing the Tetrahedral Mesh (p. ) and Refining the

Tetrahedral Mesh (p. ).

... Manual Meshing Procedure for Tetrahedral Meshes

The basic components of the manual meshing process are examining and repairing the surface mesh,

creating an initial mesh, refining the mesh, and improving the mesh.

The following steps describe the recommended meshing procedure.

Step : Examining the Surface Mesh

The first step in the mesh generation process is to examine the validity and quality of the surface

mesh. The recommended approach includes the following steps:

. Checking for free and isolated nodes (see Free and Isolated Nodes (p. )).

. Checking and improving the surface mesh quality (see Improving Boundary Surfaces (p. )).

. Visually examining the surface mesh for free, multiply-connected, skewed, and/or close-proximity faces

(see Displaying the Mesh (p. )).

. Making local repairs if required (see Modifying the Boundary Mesh (p. )).

After obtaining a valid, (ideally) high-quality surface mesh, you can proceed to create the volume mesh.

Manually Creating a Tetrahedral Mesh

Step : Creating the Initial Mesh

The first step in generating the volume mesh is creating the initial mesh. This process first creates a

pre-meshed box encompassing the entire geometry, and then sequentially introduces each boundary

node into the mesh. As the nodes of a boundary face are inserted into the mesh, any necessary mesh

modifications needed to insert the face are performed, effectively inserting both boundary nodes and

faces into the mesh simultaneously. For more information see Initializing the Tetrahedral Mesh (p. ).

Activating Multiple Zones (for Multi-zone Meshes Only)

If the mesh has multiple regions (for example, the problem requires a fluid zone and one or more

solid zones), you can refine the mesh using refinement parameters specific to individual zones, if re-

quired. The procedure for meshing multiple cell zones includes the following steps:

.

Initialize the mesh.

.

Activate the appropriate zones using the Manage Cell Zones dialog box.

.

Set the zone-specific refinement parameters and refine the active zones.

in the Tet dialog box.

Important

zones will be active after the initialization is complete. Hence, all the zones will be

considered for refinement. If required, you can change the zone type using the Manage

Note

Step : Refining the Mesh

You will refine the initial mesh by adding cells at the boundary and in the interior. The refinement

methods available are the skewness-based method and the advancing front method. You can also

define local refinement regions using the Tet Refinement Region dialog box. You can modify the

parameters in the Refinement tab of the Tet dialog box and select additional refinement options for

skewness-based refinement in the Tet Refine Controls dialog box, if required.

Step : Improving the Mesh

You can improve the skewness by smoothing, swapping, and refining the mesh further to improve

the quality of the volume mesh. At any point in the mesh generation process, you can compute and

plot the cell skewness distribution using the Cell Distribution dialog box. The number of cells in the

specified range in each of the regularly spaced partitions is displayed in a histogram format. The x

axis shows either the size or the quality and the y axis gives the number of cells or the percentage of

the total. This will give you an idea of the improvement required. It is typically possible to reduce

skewness to .–. (for simple geometries) or .–. (for more complex geometries).

Note

If you have used domains to generate the mesh or group zones for reporting (as described

in Using Domains to Group and Mesh Boundary Faces (p. )), you can report the cell dis-

tribution only for those cell zones that are in the active domain.

Step 4a: Swapping and Smoothing without Refining

Swapping and smoothing improve the mesh by manipulating the nodes and faces without increasing

the total number of cells. Refinement, on the other hand, improves the mesh by adding nodes, which

typically increases the number of cells. To get the best possible mesh with the minimum number of

cells, perform only smoothing and swapping before refining the mesh any further.

Smoothing repositions interior nodes to lower the maximum skewness of the mesh. For swapping,

given n+ nodes in dimension n, there are at most two triangulations of the nodes depending on the

configuration of the nodes. In cases where two triangulations exist, the two alternatives are examined,

and the one that has the lowest maximum skewness is selected. Smoothing and swapping are auto-

matically performed to improve the mesh when the Improve Mesh option is enabled in the Refinement

tab of the Tet dialog box.

Refer to Smoothing Nodes (p. ) and Swapping (p. ) for details on improving the mesh by swapping

and smoothing.

Step 4b: Further Refinement

You can further refine the cells in the active zones by changing parameters such as Max Cell Volume,

and Max Cell Skew and Max Boundary Cell Skew (available only for skewness-based refinement).

Important

Changing mesh size controls other than Max Cell Volume will have no effect on a mesh

that has already been refined. Alternately, use local refinement regions. Refer to Using

Local Refinement Regions (p. ) for details.

Refining with skewness parameters reduced to values less than . will rarely improve the mesh and

will be very time-consuming.

Important

Do not over-refine the mesh, the volume mesh produced should be of sufficient density to

resolve the shape and any intuitive flow features (for example, wall boundary layers). Addi-

Important

tional resolution can be more effectively produced using the solution-adaptive mesh cap-

ability provided in the solution mode in Fluent.

At this step you will have an acceptable mesh for most geometries.

Step 4c: Boundary Slivers and Other Sources of Lingering High Skewness

When viewing the cell distribution plot, if you find that there are a few cells with very high skewness,

check to see where they are located (that is, on the boundary or in the interior). To do so, use the

Report Boundary Cell Limits dialog box. When using that dialog box, note that if you have used

domains to generate the mesh or group zones for reporting (as described in Using Domains to Group

and Mesh Boundary Faces (p. )), the report will apply only to the active domain.

Refer to Removing Slivers from a Tetrahedral Mesh (p. ) and Moving Nodes (p. ) for details on

removing slivers and other mesh improvement options.

You can initialize and refine the tetrahedral mesh in a single step by clicking the Init & Refine button

in the Tet dialog box after setting the appropriate parameters in the Initialization and Refinement

tabs. Alternatively, you can set the appropriate parameters in the Initialization tab and click the Init

button to create the initial mesh. You can then refine the initial mesh by setting the appropriate

parameters in the Refinement tab and clicking the Refine button.

If you need to refine a particular region, you can define the region to be refined using the Tet Refine-

ment Region dialog box.

.. Initializing the Tetrahedral Mesh

The first step in the volume mesh generation process is initialization. The initial mesh consists of the

nodes and triangles of the boundary surface mesh. For some geometries, it is not possible to create a

tetrahedral mesh from the boundary nodes alone. In such cases, a small number of nodes are automat-

ically added in the interior of the domain. Interior nodes may also have to be added to resolve numer-

ical problems associated with the Delaunay criterion.

... Initializing Using the Tet Dialog Box

You can use Mesh → Tet to initialize the mesh using the options available in the Initialization tab of

the Tet dialog box.

.

Select the appropriate actions to be performed during initialization from the Options group box.

The Merge Free Nodes and Delete Unused Nodes options are enabled by default. You can also

include improving the surface mesh in the mesh initialization process by enabling the Improve

Surface Mesh option.

.

Select the appropriate option from the Non-Fluid Type drop-down list. Enable Delete Dead Zones, if

required.

When the initial mesh is generated, all the cells are grouped into contiguous zones separated by

boundaries. The mesh is considered to contain a single fluid zone and one or more dead regions.

The zone just inside the outer boundary is set to be active and is labeled a fluid zone. All other

non-fluid zones will be inactive. Only active zones will be considered for refinement during the

mesh generation process.

Note

Note

You can refine different groups of zones using different refinement parameters for each group

by toggling the zones between active and inactive. If however, you need to use the same refine-

ment parameters for all the zones, you can change the specification of Non-Fluid Type to a type

other than dead (for example, solid). When the Non-Fluid Type is set to a type other than dead,

all the zones will be activated after initialization. Hence, you can set the appropriate refinement

parameters without setting all the zones to be active.

.

Specify additional initialization parameters, if required.These parameters are available in the Tet Init

Controls dialog box. Click the Controls... button to open the Tet Init Controls dialog box.

.

Click Init to initialize the mesh.

A Working dialog box will appear, informing you that the initialization is in progress. Click the

Cancel button in the Working dialog box to abort the mesh initialization process. Canceling the

initialization will leave the mesh incomplete.

If you try to initialize the mesh after canceling an initial attempt, a dialog box will ask if it is OK to clear

the incomplete mesh.

After you approve, the initialization process will begin again.

If you try to initialize the mesh when duplicate nodes exist, the initialization will fail.You must clear

the mesh and merge the duplicate nodes before attempting the initialization again.

If you try to initialize the mesh when a volume mesh already exists, a Question dialog box will appear,

asking if you want to clear the existing mesh. If you click Yes, the volume mesh will be cleared and

then the mesh will be initialized. If you click No, the operation will be canceled.

If you need to preserve the existing mesh during the meshing process, use the command

/mesh/tet/preserve-cell-zone to specify the cell zones to be preserved and click the Init

button to proceed with the initialization.

If the initial mesh generation fails, check the validity of the surface mesh. In some rare cases, you may

need to change the sliver size parameter (by using the Tet dialog box).

Refer to Common Tetrahedral Meshing Problems (p. ) for more information on meshing problems.

.. Refining the Tetrahedral Mesh

After initializing the mesh, you can improve the quality and density of the mesh using global and local

refinement. Global refinement enables you to refine all cells in the active zones, while local refinement

enables you to refine cells within a specified region.

Refining the Tetrahedral Mesh

In most applications, you will use only global refinement to create an acceptable discretization of the

volume. Local refinement is used to modify the grading away from boundaries or increase the resolution

of an interior region of the mesh. You need to define and activate the regions to be refined before

The refinement process includes a series of sweeps through a sequence of sorting, refining, reverse

sorting, and swapping and smoothing of the cells. You can specify the number of refinement levels to

be performed for skewness-based refinement. Each refinement level consists of two iterations through

the refinement procedure. For each subsequent level of refinement, the cell skewness thresholds are

lowered. Additional refinement levels will increase the mesh resolution (and the number of cells) and

decrease the average cell skewness. The preset refinement control parameters are available in the Tet

Refine Controls dialog box. Alternatively, you can select the advancing front refinement method.

Specify whether the mesh has to be improved or if the slivers have to be removed during refinement.

The Improve Mesh option performs additional smoothing and swapping with lowered skewness thresholds,

attempting to improve the average skewness of the mesh.

The Remove Slivers option attempts to lower the maximum skewness by improving highly skewed (sliver)

cells.There are two approaches for sliver removal: fast and aggressive. Both methods use the same controls

and give similar results for good quality surface meshes. In case of poor surface meshes (meshes with large

size difference between neighboring elements, narrow gaps with widely varying mesh sizes on either side

of the gap, and so on), the aggressive method will typically succeed in improving the mesh to a greater extent,

but it may be slower than the default fast method.

The aggressive method corresponds to the Improve option in the Tet Improve dialog box.

The boundary mesh is fixed during the mesh improvement and sliver removal operations.

Refinement Controls

The refinement controls for the skewness method are available in the Tet Refine Controls dialog box.

Click the Controls... button in the Refinement tab of the Tet dialog box to open the Tet Refine Controls

The refinement controls for the advancing front method are available in the /mesh/tet/con-

trols/adv-front-method menu. The /mesh/tet/controls/adv-front-method/skew-

improve/target? command is important as it enables you to enable targeted skewness-based re-

finement for the advancing front method. The refinement process will attempt to reach the targeted

skewness (specified by the command /mesh/tet/controls/adv-front-method/skew-im-

prove/target-skew). Though the default values work well in most situations, it may be advantageous

to increase the target-skew value in some cases (for example, cases where a combination of a poor

surface mesh and narrow gaps will result in poor cells in the mesh) to increase the meshing speed.

... Using Local Refinement Regions

... Refinement Using the Tet Dialog Box

A refinement region limits refinement to specific cells inside the domain. When you use the Refine

option in the Tet Refinement Region dialog box, the cells within the activated regions are refined.

The primary use of refinement regions is to reduce the cell size in the region to less than it would be

normally. Currently, the only possible region shape is a box, which can be oriented as required.

The region is defined by an x, y, and z range and its orientation about the x, y, and z axes. Any cell

within the region or that intersects the region will be subjected to the refinement criteria. You can

control the concentration of interior nodes by specifying the maximum cell volume in the refinement

region. It is possible to save different values for the Maximum Cell Volume when you save each region.

You can also specify an outer region with the required volume growth to have a smooth transition

between the original and the refined cells.

Note

In addition to the use of refinement regions for refinement during the mesh generation

process, they can also be used as a postprocessing tool to refine a region of an existing

mesh.

You can create multiple regions that overlap each other and the geometry. To create additional regions,

you can copy an existing region and then modify the parameters as required. The default region includes

the entire geometry.

Figure . : Local Refinement Region for the Tetrahedral Mesh (p. ) shows the refinement region

and outer region. The maximum cell size for the refinement and outer regions is displayed based on

the maximum cell volume and outside volume growth specified. For information on refining triangular

boundary faces in anticipation of local refinement, refer to Refining the Boundary Mesh (p. ).

Figure . : Local Refinement Region for the Tetrahedral Mesh

You can use Mesh → Tet to refine the mesh using the options available in the Refinement tab of the

Tet dialog box.

.

.

Select the appropriate refinement method from the Refine Method drop-down list.

.

Enable the appropriate options in the Options group box.

.

Specify an appropriate value for Max Cell Volume.

.

Select the appropriate option from the Cell Sizing drop-down list.

Ensure that the cells in the interior are not larger than the size required by selecting the appropriate

option in the Cell Sizing list. The following options are available:

geometric

specifies that the cell size in the interior of the domain is obtained by a geometric growth from the

closest boundary according to the growth rate specified.

size-field

specifies that the cell size is determined based on the current size-field.

Note

Additional cell sizing options (none (for skewness-based refinement only) and linear)

are available only via text commands. See the Text Command List for details.

.

Modify the refinement control parameters, if required.

For the skewness method, click the Controls... button to open the Tet Refine Controls dialog box.

Select the appropriate option from the Preset Parameters drop-down list.Verify the parameter values

in the Tet Refine Controls dialog box and modify the values as appropriate.

For the advancing front method, use the commands available in the /mesh/tet/controls/adv-

front-method menu.You can also specify the targeted skewness for the refinement process (see

Refinement Controls (p. ) for details).

.

To refine specific regions of the mesh, click the Local Regions... button to open the Tet Refinement

.

Region dialog box. Define the refinement regions and activate them.The number of activated regions

will be reported in the Message field in the Refinement tab of the Tet dialog box.

.

Click Refine to refine the mesh.

.. Common Tetrahedral Meshing Problems

Most problems with the mesh generation process become manifest in the failure to generate an initial

mesh. There are two sources of such problems:

An invalid surface mesh

Incorrect sliver size specified

Some of the common problems and suggestions for checking and fixing the mesh are described in this

section.

To look at the nodes and faces that have not been meshed, enable Unmeshed in the Display Grid

Duplicate Nodes or Faces

Some codes create multiple copies of the same node where two boundary curves or surfaces meet,

resulting in a connectivity problem. This problem can be detected by reporting the number of free

nodes or by drawing the free edges. If the geometry does not contain infinitely thin walls then there

should not be any free nodes or edges. You can remove duplicate nodes using the /boundary/de-

lete-duplicate-nodes command.

The presence of duplicate faces can be detected in one of two ways:

If the nodes of the duplicate faces are not shared by the non-duplicate faces, the duplicate faces may have

free edges that can be displayed.

If the nodes are not distinct or have been merged, there will be multiply-connected edges.

Note

Duplicate faces can be handled, it is not necessary to remove them.

Extra Nodes or Faces

Note

Nodes that are not used by any face are called unused nodes. The unused nodes can easily be found

and deleted using the Merge Boundary Nodes dialog box, if those nodes are not required. However,

there are cases where these additional nodes may be useful (see Inserting Isolated Nodes into a Tet

Mesh (p. )). Extra faces can be identified and removed using the method described for duplicate

faces.

To merge nodes that are not on a free edge, in the Merge Boundary Nodes dialog box disable Only

Free Nodes in the Compare... or With... group box or in both group boxes. For example, if you read

a hybrid mesh containing hexahedral cells (and quadrilateral boundary faces) and triangular boundary

faces, there may be some duplicate nodes on adjacent quadrilateral and triangular boundary zones. To

merge them, compare free nodes on both zones with all nodes on both zones (that is, select both zones

in the Compare... and With... group boxes, and disable Only Free Nodes in one of them).

If there are intersecting faces in the mesh, you will not be able to generate a mesh until the problem

faces are removed. Most intersecting faces can be located using the /boundary/mark-face-inter-

section command. If intersecting boundary faces are encountered during initialization, a message

will be displayed.

After the meshing fails, the unmeshed faces can be drawn to see the problem area. Usually, because

the intersecting face will have been meshed, it will not be drawn and some additional sleuthing will

be required. Draw all the faces near the unmeshed faces by setting display bounds (by using the Display

Grid dialog box). Click the Mark button in the Intersect Boundary Zones dialog box to highlight the

face intersection. Alternatively, you can use the command /boundary/mark-face-intersection

to highlight the face intersection. When you set the Feature Angle, note that this specifies the minimum

angle between the feature edges that should be preserved during retriangulation. All the edges in the

zone having feature angle greater than the specified Feature Angle are retained. This option is useful

for preserving the shape of the intersecting boundary zones. A value in the range of –° is recom-

mended; a large value may distort the shape of the intersecting boundary zones.

Common Tetrahedral Meshing Problems

Poor Boundary Node Distribution

Some meshing problems can be caused by a poor quality surface mesh. The surface mesh may have

highly skewed faces, or two or more boundaries in close proximity may have very different face sizes.

In the latter case, the boundaries can be connected (for example, in a corner) or completely separate.

Either way, the boundary mesh cannot be created without considering the impact of other nearby

If the gap between two boundaries is D, the largest edge on a face should not exceed D. The mesh

quality is extremely important when a coarse mesh is required in a small gap.

Non-Closed Boundaries

You can generate an initial mesh even if there is a hole in a boundary either due to missing faces or a

gap between two zones. In this case, instead of having two separate zones on opposite sides of the

boundary, you will have just one combined zone. This situation is evident because you will have very

few zones.

If the hole is in the outer boundary, the cells outside the boundary will be combined with the cells inside,

resulting in an error.The edges around the hole will be marked as free edges and therefore can be displayed.

If the problem is caused by a small gap between boundaries and the duplicate nodes have already been

merged, increase the tolerance and perform additional merging.

The following command can be used to detect holes in the geometry by tracing the path between the

two specified cells:

/mesh/tet/trace-path-between-cells

A path between the selected cells will be highlighted.

Interior Node Near Boundary

During refinement, a node may be placed too close to a boundary face, resulting in a highly skewed

cell. You can detect this situation by displaying the highly skewed cells. You can then smooth the mesh

to eliminate the problem.

If the interior node is constrained by the boundary faces, increase the Min Boundary Closeness (in the

Tet Refine Controls dialog box) and regenerate the mesh.

Chapter : Generating the Hexcore Mesh

Hexcore meshing is a hybrid meshing scheme that generates axis-aligned Cartesian cells inside the core

of the domain and tetrahedral cells close to the boundaries. Hanging-node (or H-) refinements on the

Cartesian cells enable efficient cell size transition from boundary to interior of the domain. This results

in fewer cells with full automation and can handle complex geometries, internal walls and gaps.

The hexcore meshing scheme is applicable to all volumes but is useful mainly for volumes with large

internal regions and few internal boundaries such as intrusions or holes. The Hexcore submenu contains

options to control the hexcore mesh generation. The starting point is a valid surface mesh.

.. Hexcore Meshing Procedure

.. Using the Hexcore Dialog Box

.. Controlling Hexcore Parameters

You can control the general shape, size, and density of the core, as well as the size of elements created

at the outer boundary of the core using the parameters in the Hexcore dialog box and the commands

in the /mesh/hexcore/ menu.

There are two approaches available for generating the hexcore mesh.

The default Cartesian type.

The Octree type which supports the size controls defined, or the computed size field.This results in faster

hexcore mesh generation. However, it does not support generation of hexcore mesh up to boundaries.

When the Cartesian type is used, internally the following steps are taken to generate the hexcore mesh:

. Generating initial Cartesian cells inside a bounding box (or the region specified) around the volume to be

meshed.

. Marking both, the Cartesian cells that intersect the boundary mesh and those cells having sizes larger than

the average size of the faces they intersect.

. Marking additional buffer-layer cells adjacent to the cells marked in Step  (if specified).

. Marking additional cells to enforce one-level refinement difference between adjacent cells.

. Subdividing all marked (in steps –) cells and repeating steps – until the local face size criteria is met.

. Deleting cells that intersect or are within some distance to the closest face on the surface mesh.

. Triangulating the external surface of the hexcore by converting quads into tri interface faces.The quad

faces become parents (with type parent-face) of the interface faces.

Note

Pyramids are not used for the transition from the hexcore to the tetrahedral cell regions.

. Smoothing the interface faces (if interface smoothing is enabled).

. Initializing and refining the tetrahedral cells between the interface faces and the boundary mesh.

Note

The maximum skewness reported at the end of the refinement process is not necessarily

the final maximum skewness. Sliver cells on the interfaces can be removed at a later

stage.

. Removing sliver cells on the interface faces.

. Merging Cartesian cells with tetrahedral (and wedge, if present) cells to form contiguous cell zones.

When the Octree type is used, internally the following steps are taken to generate the hexcore mesh.

. A uniform Octree domain is initialized for the region specified by the volume to be meshed.

. The octants are refined to local surface mesh sizes and to respect BOI size controls, if defined.

If the size-field exists, the Octree refinement will be driven by the size-field instead.

. Peel layers are enforced. Cells that intersect the surface mesh or are within some distance to the surface

mesh are deleted.

. Buffer layers are enforced as applicable.

. The external surface of the hexcore mesh is triangulated, the quads are converted to tri interface faces.

The quad faces become parents (with type parent-face) of the interface faces.

Note

Note

. The interface faces are smoothed (if interface smoothing is enabled).

. The tetrahedral cells between the interface faces and the surface mesh are generated.

. The sliver cells on the interface faces are removed.

Generating the Hexcore Mesh

. The hex cells are merged with tetrahedral cells to form contiguous cell zones.

Important

If prism parameters have been attached to boundary zones, the prism layers will first be

generated. The hexcore meshing procedure will then be applied to the resulting prism caps,

along with the other boundary zones that were not involved in the prism mesh generation.

To create a hexcore mesh using the Hexcore dialog box, do the following:

.

Read in a boundary mesh and check and improve its quality, if necessary.

.

(optional) Split any quad faces in the boundary mesh into triangular faces using the /bound-

ary/remesh/triangulate command.

By default, quad faces are not allowed while initializing the hexcore mesh.

Alternatively, use the command /mesh/non-conformals/controls/enable? to enable the

creation of a non-conformal interface.

If this option is enabled, all the surfaces having quad elements will be copied and remeshed with

triangular faces. The free nodes of the triangular mesh will be merged with the original surface

mesh. The method to be used for retriangulation can be specified using the command /mesh/non-

conformals/controls/retri-method.

The quad-split method is the default method used for retriangulation. You can select prism,

quad-split, or remesh as appropriate.

.

Select the appropriate option in the Type list.

.

Specify the hexcore parameters.

Some parameters (maximum cell length or minimum cell length) required during the hexcore

meshing are automatically calculated. The hexcore meshing parameters can be changed using the

Hexcore dialog box or using the commands in the /mesh/hexcore text menu.

Note

Some operations, such as Hexcore only, are not available for object-based volume

meshing. Similarly, options under the Zones group in the Hexcore dialog box, that re-

quire a zone-based workflow, have no effect for object-based volume meshing.

.

Click Create in the Hexcore dialog box to generate the hexcore mesh.

Using the Hexcore Dialog Box

The parameters that control the hexcore mesh generation can be changed using the Hexcore dialog

box. The following options are available:

... Maximum or Minimum Cell Length

... Buffer Layers

... Peel Layers

... Defining Hexcore Extents

... Only Hexcore

... Local Refinement Regions

The use of Maximum or Minimum cell length is determined by your choice of Type.

When using the Cartesian type, the Max Cell Length is used for generating the initial Cartesian cells.

An optimal maximum cell length can be automatically calculated for a particular mesh. Click the

Compute button next to the Max Cell Length field to obtain the optimal maximum cell length for

the mesh. Alternatively, specify the maximum cell length as required.

When using the Octree type, the Min Cell Length as set by the global minimum size for scoped sizing is

used for generating the hexcore mesh.

Note

Changing the default Min Cell Length value will change the global minimum size for

scoped sizing as well.

If a size-field has been computed, the minimum cell length will be the global minimum size specified

for the size-field.

The Cartesian cells are marked (and subsequently subdivided) to satisfy the size requirement on the

boundary mesh. When there is large disparity in size distribution between the boundary mesh and

the initial Cartesian cells, there will be a rapid transition from fine to coarser cells. To avoid this, addi-

tional layers of cells are marked adjacent to those marked by the size requirement (see Figure . : Hex-

core Mesh Using (A) Buffer Layers =  (B) Buffer Layers =  (p. )). You can control the number of

additional layers by setting the Buffer Layers in the Hexcore dialog box. The default number of buffer

layers is set to . Setting the number of buffer layers to zero may result in a poor quality mesh.

Figure . : Hexcore Mesh Using (A) Buffer Layers =  (B) Buffer Layers =

Note

If the size-field has been computed and the Octree type is used to generate the mesh, the

hexcore mesh size is driven by the size-field. In this case, the number of buffer layers is not

required.

The peel layers control the gap between the hexahedra core and the geometry. After the Cartesian

required.

cells are subdivided to meet the size requirement, the cells intersected by boundary mesh and those

within some distance to the closest face on the boundary mesh are deleted. The default value for Peel

Layers is , hence this distance is assumed to be the height of an ideal tetrahedral cell on the

boundary face. If Peel Layers is set to , the gap size can be smaller than the ideal height. The resulting

hexcore mesh will contain the maximum number of Cartesian cells possible for the chosen parameters.

Figure . : Hexcore Mesh Using (A) Peel Layers =  (B) Peel Layers =  (p. ) shows the hexcore mesh

generated for different values of Peel Layers.

Figure . : Hexcore Mesh Using (A) Peel Layers =  (B) Peel Layers =

Controlling Hexcore Parameters

When using the Cartesian type, you can choose to create the hexcore mesh up to the boundary of

the domain instead of creating a tetrahedral mesh at the boundary. The hexcore mesh extents can be

defined by specifying a box in which the hexcore mesh is to be generated and/or a set of axis-aligned

planar boundaries to which the hexahedral core is to be extended. The extents can be defined as follows:

.

Enable Define Hexcore Extents in the Hexcore dialog box.

.

Click the Specify... button to open the Outer Domain Parameters dialog box.

.

Enable Coordinate Extents in the Outer Domain Parameters dialog box.The minimum and maximum

domain extents will be automatically updated with values slightly greater than the bounding box of the

surface mesh in the domain.The coordinate extents of the hexcore outer box can also be specified as

required.

Important

required.

Important

The hexcore mesh will extend to the defined domain extents. A warning will be dis-

played if the gap between the user-defined domain extents and geometric boundaries

is less than % of size of the bounding box which contains the given geometry.

.

Enable Draw Outer Box and click Draw to verify that the domain extents are correctly defined.

.

Click Apply in the Outer Domain Parameters dialog box.

.

Create the hexcore mesh.

This feature is useful for the hexcore mesh generation for external flow domains (for example, external

aerodynamics cases where the boundary conformity is not needed for far-field boundaries). This also

helps increase the count of hexahedral cells in the mesh.

In Figure . : Hexcore to the Far-Field Boundary (p. ), the hexcore mesh has been extended until

the domain boundary and does not have a tetrahedral mesh at the far-field boundary.

Figure . : Hexcore to the Far-Field Boundary

.... Hexcore to Selected Boundaries

You can use the Boundary Extents option in the Outer Domain Parameters dialog box to imprint

quad faces on selected axis-aligned planar boundaries. The selected boundary will be replaced with

a mix of quad- and tri-face zones. You can generate the hexcore mesh to selected boundaries as follows:

.

.

.

Enable Boundary Extents in the Outer Domain Parameters dialog box and select the appropriate

planar, axis-aligned boundaries to which the hexcore mesh is required.

Note

The planar boundaries must be split into separated boundary zones.

Note

The hexcore box coordinates will automatically snap to the selected boundaries.

Enable Draw Outer Box. Draw the outer box along with the selected boundaries to verify that

the box snaps to the selected boundaries.

If the box does not snap to a selected boundary, it indicates that the hexcore mesh cannot be

grown to the boundary. If the selected boundary zone is a plane which is misaligned with the

axis, you can align it using the Auto Align option as follows:

a.

Select the zones to be aligned in the Boundary Zones selection list.

The Auto Align group box will now be activated.

b.

Enable Auto Align.

c.

The recommended auto align tolerance value can be computed for the selected set of boundary

zones. Click Compute to determine the recommended tolerance or enter an appropriate tolerance

value.

d.

Click Apply in the Auto Align group box to align the selected zones which are within the tolerance

specified.

Warning

The Auto Align option may deform the geometry permanently. Take care while

selecting the boundary zones.

e.

Draw the outer box along with the selected boundaries to verify that the box has snapped to the

selected boundaries.

.

Enable Delete Old Face Zones, if required and click Apply in the Outer Domain Extents dialog box.

.

The newly created quad face zones will be named with the original zone names.

The hexcore mesh will extend to the selected boundaries, aligned with the X, Y, and Z axes. An example

is shown in Figure . : Hexcore to Boundaries (p. ).

Warning

Warning

If you attempt to use this option when the geometry is completely within the domain, an

Figure . : Hexcore to Boundaries

When using the Cartesian type, the Only Hexcore option enables you to prevent the automatic creation

of the tetrahedral mesh after hexcore generation (see Figure . : Only Hexcore (p. )). However, the

tetrahedral mesh domain is created and activated during the hexcore meshing procedure. You can

manually create the tetrahedral mesh in a separate step.

Figure . : Only Hexcore

Hex cell islands may be created when the Only Hexcore option is used. You can delete small islands

which may be created by setting the minimum allowable size for the hex cell islands using the command

/mesh/hexcore/controls/post-relative-island-count. This command is available only

when the Only Hexcore option has been enabled in the Hexcore dialog box. You can also use the

command /mesh/hexcore/controls/only-hexcore? to enable only hexcore meshing.

The default value for post-relative-island-count is . All hex cell islands whose size is less

than the specified percentage (in the default case, %) of the largest hex cell zone will be automatically

deleted.

No islands will be removed if you set the value to .

Note

This option is not available for object-based volume meshing.

Warning

You may need to verify that hex cells are created only in the domain of interest as the

mesher cannot identify whether the cells are within the domain without tetrahedral

Warning

meshing. Also, all the non-fluid type zones are created as separate fluid zones. You need

to retain the fluid zones of interest and delete the others.

When using the Cartesian type, you can use local refinement regions to refine specific cells within

the domain. During the hexcore meshing procedure, the cells within the activated local refinement

regions will be refined. Currently, the only possible region shape is a box, either aligned with the co-

ordinate axes, or oriented as required.

The region extents are defined by the center and the length of the region. The cell size within the region

can be manipulated by setting the level of refinement relative to the maximum cell length in the

hexcore domain. You can also orient the region as required. You can create multiple regions that

overlap each other and the geometry. To create additional regions, you can copy an existing region

and then modify the parameters as required. The default region includes the entire geometry.

You can use the Draw button in the Hexcore Refinement Region dialog box to display the defined

region. Figure . : Local Refinement Region for the Hexcore Mesh (p. ) shows a refinement region

defined. A sample Cartesian cell with the specified Max Length is also displayed at the center of the

refinement box.

Figure . : Local Refinement Region for the Hexcore Mesh

Chapter : Generating Polyhedral Meshes

Polyhedral meshes contain polyhedral cells. An advantage that polyhedral meshes have shown relative

to tetrahedral or hybrid meshes is the lower overall cell count, almost - times lower for unstructured

meshes than the original cell count. Since the polyhedral mesh has a lower cell count than the equivalent

original tetrahedral mesh, solution convergence will generally be faster, possibly saving some compu-

tational expense.

Polyhedral meshes can be generated using the object-based volume meshing approach. The starting

point is a valid surface mesh (see Surface Mesh Processes (p. )).

Prerequisites for generating a polyhedral mesh include:

A valid surface mesh must be a triangular mesh of good quality.

Surface triangulation size should not exceed material thickness.

The aspect ratio of prisms should be less than .

Note

The polyhedral meshing process changes triangle faces in the surface mesh to hexagonal

faces. Once the polyhedral mesh exists, you cannot regenerate the volume mesh unless you

first select the Restore Faces option. When you select Restore Faces, the current object

face zones and cell zones are deleted. You can then begin the volume meshing process again

using the original valid surface mesh as the starting point. See Generating the Volume

Mesh (p. ) for more information about Restore Faces.

The process followed and steps required to generate the polyhedral mesh are explained.

.. Meshing Process for Polyhedral Meshes

.. Steps for Creating the Polyhedral Mesh

The Auto Mesh dialog box contains options for setting up and generating a polyhedral mesh from a

valid surface mesh for all computed volumetric regions of the mesh object.

If enabled, the prism mesh is generated based on the scoped prism settings specified. Polyhedral meshing

does not support zone-specific prisms.

The polyhedral meshing process starts by generating a tetrahedral mesh in two stages: initialization and

refinement.

– The automatic initialization procedure includes the following steps:

. Improving the surface mesh based on polyhedra-driven criteria.

The cell zones are then associated with the regions and the cell zone type will be applied. Dead

cell zones will be deleted.

– The refinement procedure includes the following steps:

. Inserting nodes for refining the mesh.

. Two stages of tet mesh improvement.

The polyhedral mesh is created as a dual of the tetrahedral mesh, such that the vertex of the mesh-element

(tetrahedron) is close to the center of the solver-element (polyhedron).Tessellations are created for the

boundary and cell zones.When prism mesh is generated, the dual is used directly, meaning the layering

structure of the mesh is maintained.

The polyhedral mesh is improved by operations like merging short edges and splitting cells. Concave cells,

concave boundary faces, and stair-stepped poly cells are split to improve quality.The quality is further im-

proved by smoothing.

The best quality measures for polyhedral meshing are squish and ortho skew. If you select squish or

ortho skew, skewness evaluations during smoothing will be supplemented with additional internal

measures. If you select a quality measure other than squish or ortho skew, mesh generation will use

an internal variant of squish because it provides some direct control over the convexity of the cell.

The Auto Mesh dialog box contains options to control the polyhedral volume mesh generation.

You can generate the poly mesh as follows:

.

Open the Auto Mesh dialog box from the context-sensitive menu available by right-clicking on any mesh

object or its Volumetric Regions or Cell Zones branch in the tree.

.

Note

If you open the Auto Mesh dialog box from the context-sensitive menu in the tree, the

Mesh Object to which the cell zones or volumetric regions belong is automatically selec-

ted.

.

Enable/disable the Keep Solid Cell Zones option, as appropriate.

Generating Polyhedral Meshes

.

box.

a.

approach.

b.

Tip

Tip

Note

Stair-stepping will occur in regions of transition between the prism layers and the adja-

cent tets.

.

Set the Poly mesh parameters.

Select the Poly option from the Volume Fill list and set the following Volume Fill Options.

– Geometric specifies that the cell size in the interior of the domain is obtained by a geometric growth

from the closest boundary according to the growth rate specified.

Specify the Max Cell Length. Click Compute to compute the maximum cell size based on the mesh

object.

Note

You can also set these parameters in the Poly dialog box.

Click the Set... button to open the Poly dialog box.

a.

Select the options in the Options group box.

The Merge Free Nodes, Delete Unused Nodes, and Improve Poly Mesh options are enabled

by default. You can also include improving the surface mesh by enabling the Improve Surface

Mesh option.

Steps for Creating the Polyhedral Mesh

b.

Specify an appropriate value for Feature Angle.This sets the threshold for preserving features.The

default setting is  degrees.

c.

Select the appropriate cell zone type from the Non-Fluid Type list in the Poly Zones group box.

Note

Dead cell zones will be automatically deleted after the mesh is initialized.

When the initial mesh is generated, all the cells are grouped into contiguous zones separated

Note

by boundaries. The mesh is considered to contain a single fluid zone and one or more dead

regions. The zone just inside the outer boundary is set to be active and is labeled a fluid zone.

All other non-fluid zones will be inactive. Only active zones will be considered for refinement

during the mesh generation process.

Note

Volume region type is used to determine the cell zone type.

by toggling the zones between active and inactive. If however, you need to use the same re-

finement parameters for all the zones, you can change the specification of Non-Fluid Type

to a type other than dead (for example, solid). When the Non-Fluid Type is set to a type

other than dead, all the zones will be activated after initialization. Hence, you can set the ap-

propriate refinement parameters without setting all the zones to be active.

d.

In most cases, the default node spacing threshold should be acceptable. If you want to change it,

click Controls to open the Poly Init Controls dialog box where you can modify the value.

e.

Set poly cell growth parameters using the options in the Cell Size group box. Specify appropriate

values for Max Cell Volume and Growth Rate.You can use the Compute button to determine the

maximum cell size based on the size field.

Ensure that cells in the interior are not larger than the size required by selecting the appropriate

option in the Cell Sizing list:

geometric

specifies that the cell size in the interior of the domain is obtained by a geometric growth from

geometric

the closest boundary according to the growth rate specified.

f.

Click the Local Regions button to access the Tet Refinement Region dialog box, where you can

setup and activate local tetrahedral refinement regions.These regions are used during the initial

tetrahedral mesh generation; they are not directly applicable to the poly mesh.The number of activ-

ated regions will be reported in the Message field.

.

Return to the Auto Mesh dialog box and enable or disable additional Options as desired.

.

The prism layer cell quality distribution (see Determining Boundary Cell Quality (p. )).

The polyhedral cell quality reports (see Determining Volume Mesh Quality (p. )).

Note

The quality measure will be set to Inverse Orthogonal Quality after the polyhedral mesh

is generated.

...Transferring the Poly Mesh to Solution Mode

Node weights for node-based gradients are enabled by default for poly meshes generated in Fluent

Meshing. This setting can improve the accuracy of the displayed results near wall edges when you are

displaying contours on a native poly mesh.

When you transfer the poly mesh to solution mode, a message will notify you that this interpolation

is enabled. You can disable it by setting the /display/set/nodewt-based-interp? command

to no.

Chapter : Generating Poly-Hexcore Meshes

Poly-hexcore meshes contain polyhedral and hexcore cells. Therefore, the poly-hexcore mesh character-

istics contains elements of both types of meshes. For more information about polyhedra meshes, see

Generating Polyhedral Meshes (p. ). Likewise, for more information about hexcore meshes, see Gen-

erating the Hexcore Mesh (p. ).

.. Steps for Creating the Poly-Hexcore Mesh

The Auto Mesh dialog box contains options to control the poly-hexcore volume mesh generation.

You can generate the poly-hexcore mesh as follows:

.

.

Note

ted.

.

.

box.

a.

box.

a.

approach.

b.

Tip

.

Set the Poly-Hexcore mesh parameters.

Select the Poly-Hexcore option from the Volume Fill list and set the following Volume Fill Options.

Specify the number of Buffer Layers and Peel Layers for the poly-hexcore mesh.

Specify the Min Cell Length. Click Compute to compute the maximum cell size based on the mesh

object.

Click the Set... button to open the Poly-Hexcore Controls dialog box.

a.

Select the Avoid : Cell Jump in Hexcore option to eliminate the : cell transition that can occur

in the hexcore region.When enabled, use the Replace (With Polyhedra) drop-down menu to select

whether just large cells, just small cells, or if both types of cells are to be replaced with polyhedra

cells in the hexcore transition.

You can also use the corresponding text command: mesh/poly-hexcore/con-

trols/avoid-:-cell-jump-in-hexcore.

b.

Select the Mark Core Region Cell Type as Hex to have only hexcore cells within the core of the

volume mesh.

trols/mark-core-region-cell-type-as-hex?. The default value is yes.

c.

Select the Only Polyhedra for Selected Regions to assign polyhedra only to selective regions.This

option is available only if you have first computed your region(s).

c.

Once this option is enabled, you need to choose a specific region. For Select Regions (Largest

Region Excluded), you can choose fluid-region, solid-region, or other (Fluent automatically

excludes the largest region from the listing of available regions to choose).

When you choose other, the Selected Regions field is available so that you can specify one

or more regions. Enter the region name(s), or use the ... button to open the Volume Scope

dialog.

In the Volume Scope dialog, you can select one or more regions, using the Draw button to

visualize the regions prior to selection. Once you have selected your region(s), click OK, and

those selections will be displayed as Selected Regions in the Poly Hexcore Controls dialog.

trols/only-polyhedra-for-selected-regions. For example:

Meshing/mesh/poly-hexcore/controls> only-polyhedra-for-selected-regions

Mesh object [""] cyl*

only-polyhedra-for-selected-regions? [yes] yes

Select regions: [other]>

all-fluid-regions       other

Select regions: [other]> other

Use the following list and enter a valid region name for the mesh object "cylinder" (Largest Region Exclu

(cylinder: cylinder)

Region name [""] "cylinder"

Region name [""]

Meshing/mesh/poly-hexcore/controls>

Generating Poly-Hexcore Meshes

.

.

.

Steps for Creating the Poly-Hexcore Mesh

Chapter : Generating the CutCell Mesh

CutCell meshing is a general purpose hex-dominant meshing technique. The CutCell meshing algorithm

is suitable for a large range of applications, and due to the large fraction of hex cells in the mesh, often

produces better results than regular tetrahedral meshes. This method can be used instead of tetrahedral

or hexcore meshing, without requiring a very high quality surface mesh as a starting point. Also, this

method uses a direct surface and volume approach without the need of cleanup or decomposition,

thereby reducing the turnaround time required for meshing.

The following sections are described in this chapter:

..The CutCell Meshing Process

.. Using the CutCell Dialog Box

.. Improving the CutCell Mesh

.. Post CutCell Mesh Generation Cleanup

.. Generating Prisms for the CutCell Mesh

..The Cut-Tet Workflow

The CutCell meshing process involves the following approach:

. Objects, material points (optional), and size functions are defined.

. The initial size of the Cartesian grid is computed based on the minimum and maximum size set for the size

. A uniform Cartesian grid is created within the bounding box for the geometry.

The base size for the Cartesian grid is computed from the minimum and maximum size specified in

the Size Functions dialog box as follows:

Base Size = 2n × Min Size

such that

Base Size ≤ Max Size

where n is the number of refinement levels.

Note

You should maintain the ratio between the base size and the global minimum size such

such that

Note

that Base Size = 2n × Min Size. This ensures that the correct minimum size is used during

the CutCell meshing.

Warning

During initialization, the Cartesian grid created will contain the maximum number of

Cartesian cells possible for the computed base size. If the cell count of the initial Cartesian

grid exceeds the limit, use the command /mesh/cutcell/set/max-initial-

cells to set a more appropriate number.

. The size function values are computed and the grid is then adaptively refined based on the local size

function values.

Figure . : Schematic Representation of the Cartesian Grid Refinement Using Size Functions (p. )

shows a schematic representation of the refinement using size functions. The size source specified

via the size functions will be assimilated into the size function octree. The final mesh at respective

locations will reflect an interpolated size based on the size functions.

Figure . : Schematic Representation of the Cartesian Grid Refinement Using Size Functions

Figure . : Mesh After Refinement (p. ) shows the mesh after refining the initial grid based on

size functions.

Generating the CutCell Mesh

Figure . : Mesh After Refinement

. The cells intersected by the geometry are marked. Only nodes on marked cells are considered for projection.

The nodes are projected to the geometry (corner, edge, and face in order of reducing priority).

Figure . : Mesh After Projection (p. ) shows the mesh after node projection.

Figure . : Mesh After Projection

The CutCell Meshing Process

. The edges intersected by the geometry are identified. Mesh edges to be preserved/recovered are determined,

and are used to construct mesh faces. Once the mesh faces are identified, cells are decomposed to recover

these faces.The cells are decomposed based on a number of templates.

Note

The CutCell mesher may have problems capturing features like acute internal and external

face angles (for example, trailing edges of fins, wheel-ground intersections). If such features

are not recovered properly, the prisms generated at such locations are most likely to

have bad quality.

In such cases, you can use the set-thin-cut-edge-zones command (see Resolving

Thin Regions (p. )) and specify the edges where the feature capturing fails, and then

regenerate the mesh.

The quality of the cells thus generated is improved.

. You can set the default parameters to be used for improving the CutCell mesh using the command

/mesh/cutcell/set/set-post-snap-parameters.This command sets the quality limits and

other parameters relevant to the node movement and cavity remeshing that are performed to improve

quality.

. Cells are separated into cell zones based on the respective objects and material points (if any).When a cell

has a vertex that lies out of the object while the other lies within the object, the cell will be decomposed

further to represent the boundary crossing the cell. A cell included in multiple objects will be included with

the object having the highest priority.

Figure . : Cells Separated After Decomposition (p. ) shows the cells separated into respective

cell zones after decomposition.

Figure . : Cells Separated After Decomposition

. Dead zones are generally deleted (auto-delete-dead-zones? is enabled by default). Solid zones will

be retained or deleted, depending on the setting of auto-delete-solid-zones? (disabled by default).

. The boundary mesh is recovered and separated based on the underlying geometry.

Faces whose adjacent neighboring cells are in different cell zones automatically constitute the boundary

mesh.

The neighboring cells of a face on an internal baffle are in the same cell zone. In such cases, faces close

to and nearly parallel to the baffle surface are recovered to represent the baffle surface.

As each cell zone is a closed region, the mesh boundary is conformal.

The boundary zone types are assigned based on the underlying geometry zone type. Figure . : Cut-

Cell Mesh After Boundary Recovery (p. ) shows the CutCell mesh after the boundary mesh is re-

covered.

Note

The CutCell mesher will assign the type wall on the surface recovered over a geometry

zone of the type internal (for example, baffles) and the type geometry.

Figure . : CutCell Mesh After Boundary Recovery

The CutCell dialog box and the commands in the /mesh/cutcell menu enable you to perform

various tasks related to generating the CutCell mesh.

You can use Create in the CutCell dialog box to generate the CutCell mesh based on the objects and

material points selected.

The generic procedure for generating the CutCell mesh is as follows:

.

Define the objects.

a.

.

a.

Right click on Model in the Outline View and select Object Management... to open the Manage

Objects dialog box. See Using the Manage Objects Dialog Box (p. ).

b.

Make sure the objects are appropriately defined (see Object Attributes (p. ) for details).

c.

Create capping surfaces if required (see Patching Tools (p. ) for details).

Important

The objects defined include the corresponding edges that are used for capturing features

during the CutCell mesh generation. If you are starting from an earlier setup, you may

need to add the appropriate edge zones to the object before proceeding. Several options

for creating the Edge Zones are described in Extract Edge Zones (p. ).

.

Define the material points, if needed.

a.

Right click on Model in the Outline View and select Material Points... to open the Material Points

b.

Make sure the material points are appropriately defined (see Creating Material Points (p. ) for details).

.

Define the size functions as appropriate (see Defining Size Functions (p. ) for details).

a.

Right click on Model in the Outline View and select Functions from the Sizing context menu to

open the Size Functions dialog box.

b.

Make sure the size functions are appropriately defined.

.

Select the objects and material points to be used for the CutCell mesh generation in the CutCell dialog

box.

a.

From the Mesh menu, select Cutcell... to open the CutCell dialog box.

b.

Select the appropriate objects in the Objects selection list.

c.

Select the appropriate material points in the Material points selection list.

d.

Enable Keep Solids Cell Zones in the Options group box, if required.

c.

d.

.

Click Create in the CutCell dialog box.

The face zones are separated by cell neighbor and normals on face zones connected to the fluid

cell zones are oriented into the fluid zone. A face zone group is created for the face zones of each

fluid cell zone. Additionally, the defaults for post volume mesh prism generation will be set (see

Generating Prisms for the CutCell Mesh (p. ) for details).

.

Right click on Model in the Outline View and select Prepare for Solve.

face/cell zone name prefixes and/or suffixes, deleting unused faces and nodes are performed during

the cleanup operation.

.

Generate prism layers, if required.

a.

Click Create Prisms... to open the Prisms dialog box.

b.

Examine the face zone group created for the face zones of the fluid cell zones and determine the

face zones for which prism meshing parameters are to be specified.

c.

Specify the prism meshing parameters as appropriate and click Apply.

d.

.

Verify the quality of the CutCell mesh and perform quality improvement operations, if required.

Note

Use the File → Write → Case... menu item with the Write As Polyhedra option enabled to

write the case file in the format that can be read in solution mode in Fluent.

... Handling Zero-Thickness Walls

Certain geometries may have components that have zero-thickness. Such configurations can be handled

during the CutCell meshing process. There are two types of zero-thickness walls:

Baffles (zero-thickness walls having the same fluid/solid zone on either side)

Interior walls (zero-thickness walls having different fluid/solid zones on either side)

To allow the recovery of baffles, any such surface must be of the type internal, which will be recovered

as a wall. For jump conditions, the surface must be of one of the types fan, radiator, or porous-jump,

which will be recovered based on the type defined. All such surfaces should be included in the object

defined. If not, the surface will not be recovered.

The recovered surface for the zero-thickness baffles will be prefixed by cutcell-two-sided in the gen-

erated CutCell mesh.

Figure . : Mesh Generated for Geometry Having Zero-Thickness Baffles (p. ) shows an example

where the CutCell mesh has been generated for a stirrer geometry having zero-thickness baffles.

Using the CutCell Dialog Box

Figure . : Mesh Generated for Geometry Having Zero-Thickness Baffles

For interior walls, you can define two objects, each including the zones comprising the respective

domains. Hence, the interior wall will appear in both objects defined, and will be recovered properly.

... Handling Overlapping Surfaces

Overlapping surfaces are surfaces from independently defined objects which partially or fully overlap.

To allow the recovery of overlapping surfaces as a separate surface, the overlapping walls must be

included in both defined objects. The distance between such surfaces must be at least ten times

smaller than the minimum size set to avoid “trapped" cell zones. The overlapping surface will be included

with the recovered boundary from the object having a higher priority value.

Figure . : Recovering Overlapping Surfaces (p. ) shows an example where the CutCell mesh has

been generated for a butterfly valve. The overlapping surfaces between the valve and flow region as

well as the pipe walls and flow region are recovered.

Figure . : Recovering Overlapping Surfaces

... Resolving Thin Regions

corners, trailing edge configurations, and so on. Such configurations may not be recovered accurately

enough by the CutCell mesher, and surface elements may span between nodes on the proximal surfaces.

You can explicitly define thin regions that need to be resolved when the CutCell mesh is generated.

The command /mesh/cutcell/set/set-thin-cut-face-zones enables you to specify the

face zones constituting the thin regions to be recovered.

The command /mesh/cutcell/set/set-thin-cut-edge-zones enables you to specify edge

zones defining the features to be recovered in thin regions.

Figure . : Resolving Thin Regions (p. ) shows an example where the thin regions have been resolved

during the CutCell meshing process.

Figure . : Resolving Thin Regions

The Mesh/Tools/Auto Node Move... menu item opens the Auto Node Move dialog box, which you

can use to improve the CutCell mesh quality.

The following text commands also enable you to improve the CutCell mesh:

/mesh/cutcell/modify/cavity-remeshing

enables you to use the Cavity Remeshing utility to improve the CutCell mesh quality near the boundary.

Specify the cell zones to be improved and the quality limit as appropriate. For details on the options

available, refer to Cavity Remeshing (p. ).

Note

Face zones of type internal are recovered as type wall in the cutcell mesher. These

should be reset to type internal before using the cavity remesher.

/mesh/cutcell/modify/rezone-multi-connected-faces

enables you to resolve multi-connected configurations on the CutCell boundary. Specify an appropriate

value for the critical count for contiguous manifold faces.

An example is shown in Figure . : Rezoning Multiply Connected Faces (p. ) where the multiply

connected faces around the surface are removed.

Figure . : Rezoning Multiply Connected Faces

After generating the CutCell mesh, you can perform cleanup operations such as deleting dead zones,

deleting geometry objects, deleting edge zones, removing face/cell zone name prefixes and/or suffixes,

deleting unused faces and nodes. These operations can be performed by selecting Prepare for Solve

in the context menu under Model in the Outline View.

Note

It is recommended that you use the Delete option in the Manage Cell Zones dialog box or

the command /mesh/manage/delete to delete cell zones in the CutCell mesh, instead

of the Mesh/Clear option or the /mesh/clear-mesh command.

After generating the CutCell mesh, the face zones are separated by cell neighbor and normals on face

zones connected to the fluid cell zones are oriented into the fluid zone. A face zone group is created

for the face zones of each fluid cell zone. Additionally, the defaults for post volume mesh prism gener-

ation will be set. These include the following prism controls to reduce stair-stepping of prism layers:

Disable edge swapping.

/mesh/prism/controls/improve/edge-swap? no

Disable face smoothing.

/mesh/prism/controls/face-smooth? no

Set the skewness threshold for edge swapping and edge and node smoothing to ..

/mesh/prism/controls/improve/swap-smooth-skew .

Ensure that shrinkage for prism layers is enabled.

/mesh/prism/controls/proximity/allow-shrinkage? yes

Set the smoothing rate (rate at which shrinkage is propagated laterally) to ..

Generating Prisms for the CutCell Mesh

/mesh/prism/controls/proximity/smoothing-rate .

Disable ignoring of nodes that have poor normals.

/mesh/prism/controls/normal/ignore-invalid-normals? no

Set the cell quality criterion for smoothing and quality checking to ..

/mesh/prism/controls/improve/max-allowable-cell-skew .

Enable smoothing of normals along the feature lines of the base face zones.

/mesh/prism/controls/improve/identify-feature-line? yes

Set the maximum allowable skewness for cap faces after smoothing to ..

/mesh/prism/controls/improve/max-allowable-cap-skew .

Set the quality method to Orthoskew.

/mesh/prism/quality-method orthoskew

Enable the improvement of cell quality for every prism layer.This will involve smoothing of normals in the

current layer and perturbation smoothing to improve cell quality in the lower layer.

/mesh/prism/controls/improve/cell-quality-improve? yes

Enable the adjustment of prism heights at prism cap corners to improve cell quality.

/mesh/prism/controls/improve/corner-height-weight? yes

Disable forcible smoothing of cells if cell quality remains bad after regular smoothing.

/mesh/prism/improve/smooth-brute-force? no

You can generate prism layers on the appropriate face zones as follows:

.

Click Create Prisms... in the CutCell dialog box to open the Prisms dialog box.

.

Examine the face zone group created for the face zones of the fluid cell zones and determine the face

zones for which prism meshing parameters are to be specified.

.

Note

Hanging-node cells on a boundary for which prism generation has been assigned, will

be triangulated before the prism generation starts.

Important

Attempting to grow thicker prism layers in areas where the aspect ratio of the base to

the prism cap is very large may result in an invalid mesh. In such cases, (for example,

external flow problems) it is recommended that aspect ratio based growth be used to

avoid problems with invalid meshes.

.

As the volume mesh already exists, a Question dialog box will appear, asking if you want to morph

the existing volume mesh. Click Yes to generate the prism layers.

Alternatively, use the command /mesh/cutcell/create-prism to create the prism layers.

Specify the cell zones into which the prism layers are to be grown. The gap factor controls the

number of elements in regions of proximity.

Note

If the cell aspect ratio exceeds the specified maximum aspect ratio, a message will appear

during the prism meshing process, indicating that shrinkage was limited by the maximum

aspect ratio specified.

You could also reduce the gap factor to avoid the cell aspect ratio exceeding the specified

maximum aspect ratio. Reducing the gap factor (for example, a value of .) may improve

the quality, but could have a negative impact on the robustness of the morphing. A

higher value (for example, .) is generally more robust, but may not result in the best

mesh quality.

Note

During the surface mesh morphing, only the boundaries of face threads will be treated

as features.

When prism layers are grown into cell zones sharing a face, the prisms will be imprinted on the

shared face.

Figure . : Generating Prisms for the CutCell Mesh (p. ) shows the prism layers created for the

CutCell mesh. The prism layers will be compressed in regions of proximity and bad normals. Note

that local stair-stepping may occur in areas of poor quality.

Figure . : Generating Prisms for the CutCell Mesh

When prism layers are grown into two volumes sharing an edge, stair-stepping will occur at the common

vertex between the volumes (Figure . : Prism Growth Limitations—Volumes Sharing an Edge (p. )).

Figure . : Prism Growth Limitations—Volumes Sharing an Edge

When prism layers are grown into two volumes sharing an edge, stair-stepping will occur at the nodes

on the common boundary (Figure . : Prism Growth Limitations—Volumes Sharing an Edge (p. )).

Prism layers cannot be grown on both sides of a surface shared by adjacent volumes (Figure . : Prism

Growth Limitations—Volumes Sharing the Prism Base (p. )).

Figure . : Prism Growth Limitations—Volumes Sharing the Prism Base

A combination of node movement and cavity remeshing is carried out to improve the CutCell

mesh quality after the prism layers have been generated. The parameters for improving the

CutCell mesh quality can be specified using the command /mesh/cutcell/set/set-post-

morph-parameters prior to creating the prism layers. The quality method considered is that

set by the /mesh/cutcell/set/set-cutcell-quality-method command.

.

Ensure that the quality of the prisms created is appropriate. If the quality of the prism cells is low, you can

use post-prism smoothing to improve the quality. Use the options in the Prism Improve dialog box or

text commands such as /mesh/prism/improve/smooth-improve-prism-cells to improve

the prism cell quality.

.

To further improve the CutCell mesh using the command /mesh/cutcell/modify/post-morph-

improve, modify the relevant parameters using the command /mesh/cutcell/set/set-post-

morph-parameters.The quality considered is that set by the /mesh/cutcell/set/set-cutcell-

quality-method command.

Note

Note

This operation uses a combination of node movement and cavity remeshing to improve

the CutCell mesh quality. For details on the relevant parameters, refer to Moving

Nodes (p. ) and Cavity Remeshing (p. ).

Note

It is recommended that you use the /mesh/cutcell/modify/post-morph-im-

prove command for cell zones other than the prism cells.

The Cut-Tet workflow enables you to create a tetrahedral, hexcore, or prism mesh based on a triangulated

and improved CutCell surface mesh. The initial requirement is the generated CutCell mesh.

The generic workflow is as follows:

.

Make the CutCell boundaries conformal to remove hanging-nodes.

/mesh/cutcell/modify/split-boundary cutcell-* ,

The command /mesh/cutcell/modify/split-boundary creates a copy of the specified

CutCell boundary zones and makes the boundary mesh conformal at the hanging-nodes on the

copied zones. The new zones will be named based on the original zone names prefixed by split-.

.

Clear the volume mesh.

/mesh/clear-mesh

.

Triangulate the split CutCell boundary zones.

/boundary/remesh/triangulate split-* , yes

The split CutCell boundary zones will be replaced by the corresponding triangulated boundary

zones.

.

Improve the boundary mesh by swapping edges based on a node degree value other than .The node

degree is defined as the number of edges connected to the node.

/boundary/improve/degree-swap

Use boundary smoothing operations to further improve the boundary mesh quality (see subsequent

step).

Note

Do not use the /boundary/improve/swap operation immediately after the

step).

Note

/boundary/improve/degree-swap operation, as this will restore the original degree

configurations.

.

Improve the triangulated boundary mesh further using any of the following options available:

a.

Use wrapper smoothing operations to improve the boundary mesh quality.

i.

Change the type of the triangulated boundary mesh to wrapper.

ii.

Use the wrapper post improve operations to improve the boundary mesh quality. Refer to Dia-

gnostic Tools (p. ) or Improving the Mesh Objects (p. )for detailed descriptions of the options

Note

Make sure the original geometry is retained when the CutCell mesh is gener-

ated, this required for reprojection when using the post improve operations.

b.

Use operations like improving based on boundary mesh quality, smoothing, and swapping to improve

the boundary mesh quality. Refer to Improving Boundary Surfaces (p. ) for the detailed descriptions

of the options available.

c.

Use surface remeshing with the size functions defined for the CutCell mesh.

i.

Extract edge zones from the triangulated boundary mesh.

This enables you to maintain the boundary node locations on the remeshed faces and

facilitates the connection between the remeshed faces using simple node merge opera-

tions.

Split the edges having sizes bigger than the size function defined using the Scheme

command  (ti-refine-edge-threads-by-sf (get-edge-zones-of-filter

'split-*))

ii.

Remesh the triangulated boundary mesh using the defined size functions using the Scheme

command (ti-remesh-multiple-threads (get-face-zones-of-filter 'split-

ii.

) #f #t "none" #t)

This enables you to remesh multiple surfaces in a single operation.

Tip

You can also add a meshed size function on the edge zones extracted from

the triangulated boundary mesh to improve the quality.

iii.

Merge duplicate boundary nodes on the remeshed boundary zones.

.

Generate the tetrahedral/hexcore/prism mesh. Refer to Generating Tetrahedral Meshes (p. ), Generating

the Hexcore Mesh (p. ), and Generating Prisms (p. ) for the detailed descriptions of the meshing

The Cut-Tet Workflow

options available.You can also use the Auto Mesh option (see Using the Auto Mesh Dialog Box (p. ))

for generating the mesh.

Note

To generate the tetrahedral mesh using the defined size functions, use (tgsetvar!

'impose/cell-size-method ). This will also respect the body of influence size

functions defined for the CutCell meshing.

You can also use additional operations during the volume meshing process, as appropriate. For

example, /mesh/manage/merge-dead-zones can be used to merge dead zones having a cell

count lower than the specified threshold value, with the adjacent cell zone.

.

Improve the mesh quality using the various improvement options available. Refer to Improving the

Mesh (p. ) for detailed descriptions of the options available.

Chapter : Improving the Mesh

A volume mesh created from a high-quality surface mesh may contain some high-skewness cells. The

poor cells may result from unsuitable mesh size distribution over the domain or, more often, are caused

by constraints imposed by the boundaries.

After creating a tetrahedral or hybrid mesh, you can improve the quality of the mesh by smoothing

nodes and swapping faces. Smoothing and face swapping are tools that help to improve the quality of

the final numerical mesh. You can also use the improve command which combines operations like

collapsing cells, node smoothing, face swapping, and inserting nodes. This chapter describes the options

available for improving the mesh quality by removing highly skewed cells.

.. Smoothing Nodes

.. Swapping

.. Improving the Mesh

.. Removing Slivers from a Tetrahedral Mesh

.. Modifying Cells

.. Moving Nodes

.. Cavity Remeshing

.. Manipulating Cell Zones

.. Manipulating Cell Zone Conditions

.. Using Domains to Group and Mesh Boundary Faces

.. Checking the Mesh

.. Selectively Checking the Volume Mesh

.. Checking the Mesh Quality

.. Clearing the Mesh

Smoothing repositions the nodes to improve the mesh quality. The smoothing methods available are:

... Laplace Smoothing

...Variational Smoothing of Tetrahedral Meshes

... Skewness-Based Smoothing of Tetrahedral Meshes

Laplace smoothing is used to improve (reduce) the average skewness of the mesh. In this method, a

Laplacian smoothing operator is applied to the unstructured grid to reposition nodes. The new node

position is the average of the positions of its node neighbors.

The relaxation factor (a number between . and .) multiplies the computed node position increment.

A value of zero results in no movement of the node and a value of unity results in movement equivalent

to the entire computed increment.

This node repositioning strategy improves the skewness of the mesh, but usually relaxes the clustering

of node points. In extreme circumstances, the unchecked operator may create grid lines that cross

over the boundary, creating negative cell volumes. To prevent such crossovers, the skewness of the

resulting cells is checked before the node is repositioned. This makes the smoothing operation time-

consuming.

The smoothing operator can also be applied repeatedly, but as the number of smoothing iterations

increases, the node points have a tendency to pull away from boundaries and the mesh tends to lose

any clustering characteristics.

Variational smoothing is available only for tetrahedral meshes. It can be considered as a variant of

Laplace smoothing. The new node position is computed as a weighted average of the circumcenters

of the cells containing the node. The variational smoothing method is provided as a complement to

Laplace smoothing.

Skewness-based smoothing is available only for tetrahedral meshes. When you use skewness-based

smoothing, a smoothing operator is applied to the mesh, repositioning interior nodes to lower the

maximum skewness of the mesh. Interior nodes will be moved to improve the skewness of cells with

skewness greater than the specified minimum skewness. You can also specify an appropriate value for

the minimum improvement, if required. This allows you to stop performing the smoothing iterations

when the maximum change in cell skewness is less than or equal to the value specified for minimum

improvement.

The maximum change in cell skewness will be compared with the specified value for minimum im-

provement. When the maximum change in cell skewness is less than or equal to the value specified

for minimum improvement, further smoothing iterations will no longer yield appreciable improvement

in the mesh. The smoothing will be stopped at this point even if the requested number of iterations

has not been completed.

This skewness-based smoothing process can be very time-consuming, so it is advisable to perform

smoothing only on cells with high skewness. Improved results can be obtained by smoothing the

nodes several times. There are internal checks that will prevent a node from being moved if moving

it causes the maximum skewness to increase, but it is common for the skewness of some cells to increase

when a cell with a higher skewness is being improved. Hence, you may see the average skewness in-

crease while the maximum skewness is decreasing.

You should consider whether the improvements to the mesh due to a decrease in the maximum

skewness are worth the potential increase in the average skewness. Performing smoothing only on

cells with very high skewness (for example, . or .) may decrease the adverse effects on the average

skewness.

For tetrahedral meshes, swapping involves searching for a specific configuration of cells and replacing

it by an alternative configuration. The default option is a – swap configuration where three tetrahedra

are replaced by two tetrahedra after swapping. The other possible combinations are the – swap

configuration (replacing two tetrahedra by three) and the – swap configuration (replacing four existing

tetrahedra with four alternate tetrahedra).

Figure . : – and – Swap Configurations (p. ) shows the – and – swap configurations. The

two tetrahedra (on the left) having a common interior face can be replaced by three tetrahedra having

Improving the Mesh

a common interior edge. The common face will be replaced by three interior faces and an interior edge

during swapping. Conversely, the three tetrahedra (on the right) have two interior faces each and share

a common interior edge. During swapping for a – configuration, three interior faces and the common

interior edge will be replaced by a single face. This results in two tetrahedra having a common interior

face.

Figure . : – and – Swap Configurations

Another possible swap configuration is the – swap configuration where four tetrahedra will be replaced

by four alternate tetrahedra. In Figure . : – Swap Configuration (p. ), either the common interior

edge or two common faces can be replaced, resulting in four alternate tetrahedra.

Figure . : – Swap Configuration

Swapping

The Improve operation is an automated procedure for sliver removal or for reducing the maximum

skewness in the mesh. The improvement is carried out by removing cells above the specified skewness

threshold by collapsing cells, swapping faces, smoothing nodes, and inserting new nodes iteratively.

Each operation is specialized, and the mesh will be modified only if the mesh is noticeably improved.

The skewness before and after an operation is taken into account to determine the improvement. Hence,

the lower the skewness of the cells involved, the larger the improvement will have to be in order for

the mesh to be modified. The improve operation is a more elaborate version of the Remove Slivers

option invoked from the Refinement tab in the Tet dialog box.

A sliver typically denotes a flat tetrahedral cell. Figure . : Sliver Formation (p. ) shows an acceptable

tetrahedron.

Figure . : Sliver Formation

If the top node of the tetrahedron were to travel along the path of the dotted line in the direction of

the arrow, as it approached the end of the line the resulting cell would be a degenerate tetrahedron,

or a sliver.

In the following sections, the term sliver is used to denote all types of poorly shaped cells. There are

several commands for removing slivers or to reduce the maximum skewness of the mesh.

... Automatic Sliver Removal

... Removing Slivers Manually

Sliver removal operations can be invoked during the tetrahedral mesh refinement process. The Remove

Slivers option in the Refinement tab of the Tet dialog box controls the removal of slivers during the

meshing process. The Remove Slivers option includes operations such as collapsing cells (to remove

nodes), face swapping, smoothing, and point insertion, which are invoked iteratively.

Usually the sliver cells will be removed during refinement, but occasionally a few might be left behind.

In such cases, you can use the options in the Slivers tab in the Tet Improve dialog box to remove

the slivers manually. The Improve command uses an automated procedure to remove slivers or to

improve the mesh quality in general.

The Tet Improve dialog box contains options for removing slivers manually. The operations available

for sliver removal are as follows:

Smoothing Boundary Slivers

This operation involves smoothing nodes on sliver cells having at least one node on the boundary.

During smoothing, the nodes will be repositioned so long as the skewness of the surrounding cells is

improved. The nodes on features will also be smoothed, but will not be projected on to the original

geometry. However, nodes at branch points (more than two feature edges at the node) and end points

(one feature edge at the node) will be fixed. The nodes will be smoothed until the skewness value is

less than the specified value. The default values for the skewness threshold, minimum dihedral angle

between boundary faces, and feature angle are ., , and , respectively.

Smoothing Interior Slivers

This operation involves smoothing non-boundary nodes on sliver cells having skewness greater than

the specified threshold value. The default value for the skewness threshold is ..

Swapping Boundary Slivers

A flat boundary cell containing two boundary faces can be removed by moving the boundary to exclude

the cell from the zone in which it is located, effecting a minor change in the geometry. However, if

there is another live zone on the other side of the boundary, this operation will result in the cell being

moved to the other zone. In such cases (for example, conjugate heat transfer problems), you can decide

which live zone is least critical, and then move the boundary sliver to that zone.

The default values for the skewness threshold and the minimum dihedral angle between faces are

. and , respectively.

Refining Boundary Slivers

This operation attempts to increase the volume of boundary slivers to create a valid tetrahedral cell.

Tetrahedra having one or two faces on the boundary are identified and then the edge opposite the

boundary faces are split. The edge opposite the face pair with the largest dihedral angle will be split

for a tetrahedron with one boundary face, while the edge opposite the boundary faces will be split

for a tetrahedron having two boundary faces. The split node is then smoothed such that the volume

of the tetrahedron increases, thereby creating a valid tetrahedral cell.

Refining Interior Slivers

This operation attempts to remove the sliver by placing a node at or near the centroid of the sliver

cell. Swapping and smoothing are then performed to improve the skewness.

Removing Slivers from a Tetrahedral Mesh

Collapsing Slivers

This operation attempts to collapse the edge of a skewed sliver cell on any one of its neighbors. The

default skewness threshold is ..

Note

If you are not using a two-sided wall condition for the boundary, you can slit the face zone

containing the sliver (using the /boundary/slit-boundary-face command) and then

perform the sliver-removal operation.

Multiple slivers may exist on top of each other thus, requiring multiple operations to remove

them all.

Additional tools are available for you to perform primitive operations on the cells such as smoothing

them all.

nodes, swapping cells, splitting cells, and so on. This section describes the generic procedure for

modifying the cells using the Modify Cells dialog box. You will also use the Display Grid dialog box

during the modification of the cells.

... Using the Modify Cells Dialog Box

. Display the cells or cell zones to be modified using the options in the Display Grid dialog box.

. Select the type of entity (cell, face, node, and so on) you want in the Filter list in the Modify Cells dialog

box.

. Select the entity to be modified in the graphics window.

. Click the appropriate button in the Operation group box.

The display will be automatically updated to reflect the change made by the operation.

. Repeat the procedure to perform different operations on the cells.

Warning

Save the mesh periodically as not all operations are reversible.

The options in the Draw Cells group box enable drawing of cells using nodes or faces selected in the

Use the Using Nodes option to display cells which contain the selected nodes.

Use the Using Faces option to display cells which contain the selected faces.

The operations available in the Modify Cells dialog box for modifying cells are as follows:

The selected nodes will be repositioned based on the average of the surrounding nodes during node

smoothing. Select the nodes to be smoothed and click Smooth in the Operation group box to smooth

nodes.

Splitting Cells

The selected cell will be refined by the addition of a node at the centroid of the cell during splitting.

nodes.

Each cell will be split into four cells.

You can move the selected node either to a specified position or by a specified magnitude.

Do the following to move a node to a particular position:

.

Select node in the Filter list and select the node to be moved.

.

Select position in the Filter list and select the appropriate position.

.

Click Move To in the Operation group box.

Do the following to move a node by a specified magnitude:

.

.

Enter the magnitude by which you want to move the node in the Enter Selection field and press Enter.

The increment will now be selected in the Selections list.

.

Click Move By in the Operation group box.

Swapping Cells

You can perform either a - configuration swap or a - configuration swap. Refer to Swapping (p. )

for details on the swap configurations. Do the following to swap cells:

.

Select the appropriate option in the Filter list and select the entities to be swapped.

Select  cells or the common edge in order to perform a - swap.

Select  cells or the common face in order to perform a - swap.

.

Click Swap in the Operation group box.

Determining the Coordinates of the Centroid

Do the following to determine the centroid:

. Select the appropriate option in the Filter list (cell, face, edge, or node) and select the required entity.

. Click Centroid in the Operation group box.

Modifying Cells

The centroid coordinates will be printed in the console.

Determining the Distance Between Entities

Do the following to determine the distance between entities:

. Select the appropriate option in the Filter list and select the two entities between which the distance is

to be determined.

. Click Distance in the Operation group box.

The distance between the selected entities will be printed in the console.

You can project nodes onto a specified projection line or plane. Do the following to project nodes:

. Define the projection line or projection plane, as appropriate.

a.

Select the appropriate option in the Filter list.

b. Select two entities to define the projection line or three entities to define the projection plane.

c.

Click Set in the Operation group box to define the projection line or plane.

The line coordinates or plane position will be reported in the console.

. Select the nodes to be projected.

The projection line/plane will be highlighted in the display window.

. Click Project in the Operation group box.

Highly skewed meshes can be improved by moving the nodes of the cells. Moving nodes manually is

a time consuming process. The node movement process for improving the mesh quality is automated.

You can specify quality improvement based on the quality measure specified or based on the warp

(quadrilateral elements). You can also choose between the automatic correction procedure and the

semiautomatic correction procedure for the quality-based correction. You can also repair negative

volume cells by moving nodes using the automatic correction procedure.

... Automatic Correction

... Semi-Automatic Correction

... Repairing Negative Volume Cells

The automatic correction allows you to improve all the cells in the selected cell zone based on the

specified criteria. You can also improve the cells based on the warp values.

You can access the Auto Node Move dialog box using the Mesh → Tools menu; or by right clicking

on Cell Zones or any individual cell zone in the tree. Selecting from the tree will automatically select

the individual cell zone or all zones.

Quality-Based Improvement

For the quality-based correction, you can specify the quality limit based on the quality measure selected,

dihedral angle, and the number of iterations per node to be moved. The cells which have a quality

above the specified threshold limit will be selected.

For boundary nodes, you can restrict the node movement in the plane containing each of the

boundary faces sharing the node being moved. Nodes on sharp features and free edges will not be

considered for movement.

The node to be moved for a particular cell will be selected based on the selection of zones in the

Boundary Zones selection list and an alternative position for the node will be determined. The node

will be moved to the new position only if the quality of the cell and its neighbors is improved by the

change in node position. The procedure is repeated for the specified iterations per node. You can also

set the number of repetitions through the automatic correction procedure as required. By default, the

correction procedure is performed only once.

Warp-Based Improvement

For the warp-based correction, you can specify the maximum warp and the number of iterations per

face to be improved. The quadrilateral faces which have a warp value greater than the specified max-

imum warp will be selected. The ideal position for the node to be moved will be determined based

on the remaining three nodes. The node will be moved to the new position only if the warp of the

face decreases and the cell quality does not deteriorate by the change in node position. The procedure

is repeated for the specified iterations per face. You can also set the number of repetitions through

the automatic correction procedure as required. By default, the correction procedure is performed four

times.

The semi-automatic correction is available only for quality-based improvement. The generic procedure

for using the semiautomatic correction is as follows:

.

Select the appropriate zones in the Cell Zones drop-down list and the Boundary Zones selection list.

.

Select the quality measure and specify values for Quality Limit, Iterations/Node, and Dihedral Angle

as appropriate.

.

Enable Restrict Boundary Nodes Along Surface if required.When this option is enabled, the movement

of the boundary node will be limited to the plane containing the boundary faces sharing the boundary

node (see Figure . : Movement of Boundary Nodes (p. )).

Figure . : Movement of Boundary Nodes

.

Click Skew to display the cell with the worst quality depending on the quality limit specified.The cell

.

having the worst quality and cells/faces within a pre-defined range of the cell will be displayed.

.

Click Propose.The node to be moved and the alternative position will be highlighted.The improvement

in the skewness will also be reported in the console.

.

If the proposed position is appropriate, click Accept; otherwise, click Refuse and then Propose to obtain

the next suggestion.

.

Click Next Skew to proceed with the node correction for the next cell.

You can also repair negative volume cells by moving nodes. Specify the appropriate boundary zones,

dihedral angle, the number of iterations per node to be moved and the number of iterations of the

automatic node movement procedure (default, ). You can also choose to restrict the movement of

boundary nodes along the surface.

Cavity remeshing is useful in parametric studies because it enables you add, remove, and replace different

parts of the existing mesh. You can compare alternative designs by creating a cavity around the object

to be replaced and then, inserting the new object and connecting it to the existing mesh. Prisms can

be grown using appropriate parameters and the cavity can be filled with cells. You can also improve

the quality of the volume mesh by creating an appropriate cavity around the skewed cells and

remeshing it.

You can create a cavity in an existing mesh by removing cells in a defined bounded region. The cells

intersecting the bounded region will be marked and the cavity boundaries will be extracted from the

marked cells. The marked cells will then be deleted to create the cavity.

The various options available are:

Removing zones:This option allows you to specify zones to be removed from the existing volume mesh.

Adding zones:This option allows you to add new zones to the existing volume mesh.

Replacing zones:This option allows you to remove a set of zones and replace them with a new set of zones.

Improving a region:This option allows you to define a cavity around skewed cells in the existing mesh.You

can modify the mesh as appropriate and then remesh the cavity.

The following sections describe the cavity remeshing options:

...Tetrahedral Cavity Remeshing

... Hexcore Cavity Remeshing

The generic procedure for remeshing a cavity with tetrahedra using the Cavity Remesh dialog box is

as follows:

. Select the appropriate zones from the Remove Boundary Zones and Add Boundary Zones selection

lists.

Removing Zones: Select the zones to be removed in the Remove Boundary Zones selection list. Make

sure that no zones have been selected in the Add Boundary Zones list.

Adding Zones: Select the zones to be added in the Add Boundary Zones selection list. Make sure that

no zones have been selected in the Remove Boundary Zones list.

Replacing Zones: Select the zones to be removed in the Remove Boundary Zones selection list and

the zones to be added in the Add Boundary Zones selection list.

Improving a Region: Make sure that no zones have been selected in the Remove Boundary Zones

and Add Boundary Zones selection lists.

. Enable Create Face Group if you want to create a user-defined group (UDG) comprising the zones defining

the cavity domain.

The cavity UDG and the corresponding cavity domain will be created, but the global domain will

be retained as active when the Create Face Group option is enabled. When this option is disabled,

the cavity domain will be activated when the cavity is created.

Important

The Create Face Group option is useful when using the cavity remeshing feature for

large cases. For such cases, you can avoid frequent switching between domains by en-

abling the Create Face Group option when creating the cavity. The basic procedure is

a.

Create a UDG for the cavity and save the boundary mesh for the cavity group defined using

the File/Write/Boundaries... option (see Writing Boundary Mesh Files (p. )).

b. Read this boundary mesh in a separate session and create the volume mesh in the cavity

c.

Save the volume mesh and read it back into the previous session using the Append File(s)

option.

Cavity Remeshing

d. Connect the meshed cavity to the parent mesh and merge the cavity domain with the

parent domain.

. Enter an appropriate value for Scale and click Compute.The extents of the bounding box will be computed

(based on the zones selected in the Remove Boundary Zones and Add Boundary Zones selection lists,

and the scale factor specified) and reported in the Cavity Remesh dialog box. Alternatively, you can

specify the extents of the bounding box as required.

Warning

Warning

You need to manually specify the extents of the bounding box when using the

cavity remeshing feature to improve a region of skewed cells.

. Specify the orientation of the bounding box in the Orient group box.

. Click Draw to preview the cavity domain to be created.

. Click Create to create the cavity domain.The boundary zones touching the cavity bounding box will be

separated and included in the cavity domain along with the new zones to be added. Any zones to be re-

moved will not be included in the cavity domain.The existing volume mesh in the cavity will be removed

and boundary zones extracted from the interior zones (if any) will be changed to internal type and included

in the cavity domain.

. Connect the new zones with the boundaries of the cavity domain using node merging or intersect oper-

ations when removing, adding, or replacing zones in the volume mesh. Refer to Manipulating Boundary

Nodes (p. ) and Intersecting Boundary Zones (p. ) for details. Modify the boundary mesh (if required)

when improving a region in the volume mesh. Refer to Manipulating the Boundary Mesh (p. ) for details

on the various mesh improvement options.

. Activate the cavity domain and create the volume mesh as appropriate.

Figure . : Cavity Around a Mirror Remeshed With Tetrahedra (p. ) shows a cavity created around

the rear-view mirror of a car. You can see the original mesh and the cavity created around the

mirror and remeshed with tetrahedra. The bounding box defined for the cavity is also shown.

Figure . : Cavity Around a Mirror Remeshed With Tetrahedra

. Activate the global domain and delete the boundary zones which are no longer required. Merge the

cavity domain with the parent domain using the command /mesh/cavity/merge-cavity.

During the merging operation, the cavity cell zones will be merged with the cell zones in the parent

domain. The boundaries extracted from the interior zones will be converted to interior type and

merged with the corresponding zones in the parent domain. Other boundary zones included in

the cavity domain will be merged with the parent face zones.

The generic procedure for remeshing a cavity with a hexcore mesh using the Cavity Remesh dialog

box is as follows:

lists.

Note

Hexcore cavity remeshing is not supported for baffles/dangling walls.

Hexcore cavity remeshing is not supported if the mesh contains any dead cell zones.

Note

. Enable Hexcore Cavity to remesh the cavity with hexcore mesh.

Note

If this option is disabled, only the tetrahedral cells in the cavity will be replaced during

the cavity remeshing.

Warning

Note

The Orient group box will be disabled when the Hexcore Cavity option is enabled.

Note

Any dead cells which intersect the cavity bounding box should be converted to fluid or

solid type.

moved will be deleted from the global domain.The existing volume mesh in the cavity will be removed

ations when removing, adding, or replacing zones in the volume mesh. Ensure that the new boundaries

are properly connected with the existing boundaries. Refer to Manipulating Boundary Nodes (p. ) and

Intersecting Boundary Zones (p. ) for details. Modify the boundary mesh (if required) when improving

a region in the volume mesh. Refer to Manipulating the Boundary Mesh (p. ) for details on the various

mesh improvement options.

. If required, create the prism layers as appropriate.

Important

To facilitate easier scripting of design changes in Hexcore meshes with prism layers using

the Cavity Remeshing utility, the prism base boundary zones separated during the cavity

creation are suffixed by _cavity-prism:#. This allows you to easily identify the zones to

be assigned prism growth settings while remeshing.

. Click Remesh to create the volume mesh in the cavity.

During the remeshing operation, the cavity cell zones will be merged with the cell zones in the

parent domain. The boundaries extracted from the interior zones will be converted to interior type

and merged with the corresponding zones in the parent domain. If the remeshing involves hexcore

mesh generated to selected boundaries, the old boundaries will be removed and replaced during

the remeshing operation.

Note

Do not change domains between the Create and Remesh operations.

Figure . : Cavity Around a Mirror Remeshed With Hexcore Mesh (p. ) shows the procedure for

creating a cavity to replace the rear-view mirror of a car. You can see the original mesh and the cavity

created around the mirror. Prisms are then generated and the cavity is remeshed with hexcore mesh.

Figure . : Cavity Around a Mirror Remeshed With Hexcore Mesh

When a volume mesh is created (of any cell shape) from a boundary mesh, these cells will be grouped

into cell zones (contiguous zones separated by boundaries). You can manipulate these zones to control

further mesh generation or to duplicate an existing volume mesh to model a repeated geometry.

... Active Zones and Cell Types

... Copying and Moving Cell Zones

After the initial mesh is generated, all the cells are grouped into contiguous zones separated by

boundaries. An artifact of the meshing algorithm is that a virtual zone is created outside the outer

boundary, and it is always given a cell type of dead. This zone is automatically deleted upon completion

of the initial mesh generation. If the initial mesh generation is interrupted for some reason, this zone

will remain in the mesh until the initialization is completed. Other zone types available are fluid and

solid.

The zone just inside the outer boundary is automatically set to be active and labeled a fluid zone, al-

though you can change this type later. When refining the mesh, only the active zones are refined. By

toggling the zones between active and inactive, you can refine different groups of zones independently,

using different mesh parameters for the different groups.

If you plan to refine all cell zones using the same refinement parameters, change the Non-Fluid Type

in the Tet dialog box before initializing the mesh. If you change the Non-Fluid Type to any type

other than dead, all zones will be set active automatically after the initialization occurs. This eliminates

the need for you to set all zones to be active in the Cell Zones dialog box.

If you are creating a mesh for a geometry that repeats periodically, you can simplify the meshing tasks.

To do this, create the boundary and volume mesh for just one of the repeated sections. Copy the ap-

propriate cell zones to the required locations. If the copy shares a boundary with the original zone

(that is, if the two zones are connected), ensure that the distribution of nodes is the same on the two

overlaid boundaries.

A simplified case is illustrated in Figure . : Copying and Translating a Cell Zone (p. ). Here, the

volume mesh was created for zone , and then copied and translated to create zone . The node dis-

tribution on the left boundary of zones  and  is the same as the distribution on the right boundary.

Because the left boundary of zone  is overlaid on the right boundary of zone , there will be duplicate

nodes. It is important that you merge these duplicate nodes.

Figure . : Copying and Translating a Cell Zone

The procedure for doing this is as follows:

. Open the Merge Boundary Nodes dialog box.

. Compare all nodes on both boundaries.To do this, select the two zones in both the Compare... and

With... group boxes.

. Disable Only Free Nodes for both the zones.

. Click the Merge button to merge the duplicate nodes.

After the duplicate nodes on the two boundaries have been merged, one of the two boundary face

zones will be deleted automatically. Because duplicate faces are merged when the duplicate nodes

are merged, one zone will no longer have any faces.

the mesh information. The Cell Zone Conditions dialog box enables you to copy or clear cell zone

conditions when a case file is read.

You can copy the cell zone conditions from the zone selected in the With list to those selected in the Without

list using the Copy option.

You can clear the cell zone conditions assigned to the zones selected in the With list using the Clear option.

Manipulating Cell Zone Conditions

Domains allow you to group different boundary zones together so that you can create tetrahedral

meshes in the region they enclose, or you can limit the zones available for a display or report to only

those zones in a selected subset of the domain, rather than the entire domain.

... Using Domains

... Defining Domains

If you are generating a hybrid mesh containing hexahedra, tetrahedra, and pyramids, you can identify

a domain of the global mesh as the region in which you want to generate tetrahedral cells. You can

also use domains to group boundary zones so that you can perform diagnostics on them or display

them. When you display the grid, the zones available for display will be only those zones that are in-

cluded in the active domain. Similarly, diagnostic reports will report information about only those

zones.

If you want to check a subset of the global domain, you can create and activate a domain that includes the

desired zones, and then proceed with the display or report.

zones.

If you want your grid display or report to include all zones in the mesh, activate the global domain in the

Domains dialog box.

The procedure for defining a new domain is as follows:

. Deselect all zones in the Boundary Zones list and click Create. It is quicker to create an empty domain

and then add the zones you want, instead of creating a domain with many zones and then removing

those you do not want.

. In the Boundary Zones list, select the zones you want to include in the new domain. If you are not sure

about the zones, click Draw to display the zones that are currently selected in the Boundary Zones list.

It is possible to select all triangular or quadrilateral boundary face zones by choosing tri or quad

in the Boundary Zone Groups list.

If you are creating a domain within a hybrid mesh to create tetrahedra, make sure that the domain

contains all zones required to enclose the region that is to be meshed with tetrahedra, and only those

zones.

If the zones you select do not completely enclose the region, or if you include additional zones that do

not bound this region, the tetrahedral meshing is likely to fail or be incorrect.

. Click Change.The dialog box will be updated so that the node, face, and cell zones highlighted in their

respective lists are those that are affiliated with the boundary zones in the domain.

. Select the domain that you want to mesh (or display or report on) in the Domains list, and then click the

Activate button.This domain is then considered to be the active domain, and the Activate button is

disabled until you select another domain.

By default, the most recently created domain is automatically set to be the active domain, so you

only need to explicitly set the active domain if it is not the one you just created.

Note

If you are dissatisfied with the domain definition, delete it using the Delete button and

start over, or modify it by selecting it and using the Change button.

When you complete the mesh generation process, you need to check the mesh before saving it.

The mesh checking capability will check the mesh connectivity and the orientation of the faces (face

handedness, which should be right-handed for all faces because the solvers use a right-handed system).

The domain extents and statistics for volume and face area will be reported along with the results of

other checks on the mesh.

Mesh → Check.

The mesh check information will be printed in the console. The sample output is as follows:

Domain extents.

x-coordinate: min = -.500000e+, max = .500000e+.

y-coordinate: min = -.357625e-, max = .000000e+.

z-coordinate: min = -.111022e-, max = .000000e+.

Volume statistics.

minimum volume: .297312e-.

maximum volume: .856795e-.

total volume: .953600e+.

Face area statistics.

minimum face area: .258676e-.

maximum face area: .944555e-.

average face area: .939640e-.

Checking number of nodes per edge.

Checking number of nodes per face.

Checking number of nodes per cell.

Checking number of faces/neighbors per cell.

Checking cell faces/neighbors.

Checking isolated cells.

Checking face handedness.

Checking periodic face pairs.

Checking face children.

Checking face zone boundary conditions.

Checking for invalid node coordinates.

Checking poly cells.

Done.

The domain extents list the x, y, and z coordinates in meters.

The volume statistics include the maximum, minimum, and total cell volume in m3. A negative value

for the minimum volume indicates that one or more cells have improper connectivity. The negative

volume cells should be eliminated before the computing the flow solution.

The face area statistics include the maximum, minimum, and average face area in m2. A value of zero

for minimum face area indicates that one or more cells have degenerate faces. The mesh check may

also fail if cells have faces with very small non-zero face areas. Such cells should also be corrected before

computing the flow solution.

Checking the Mesh

The topological information verified includes the number of nodes and faces per cell. A tetrahedral cell

should have  faces and  nodes while a hexahedral cell should have  faces and  nodes.

Next, the face-handedness and face node order for each zone will be checked. The zones should contain

all right-handed faces and all faces should have the correct node order. Besides this, the mesh check

report will also display warnings based on the results of the checks previously described. If any problems

are reported, you need to repair the mesh.

Note

After creating a volume mesh, it is important to perform a thorough check of the mesh in order to ensure

that the mesh is valid. In some cases, you might prefer to have more control over what aspects of the

mesh are checked, or you may wish to perform the mesh check on specific zones, rather than all zones.

To selectively check the volume mesh, use the corresponding option available under the Mesh menu.

Mesh → Selective Check

This displays the Selective Mesh Check dialog where you can have more flexibility and more granular

control over the mesh check procedure and scope.

Figure . : The Selective Mesh Check Dialog

. Select one or more cell zones from the Cell Zone list.

. Alternatively, you can select one or more groups of cell zones from the Cell Zone Groups list.

. From the Parameters group, select specific items from the list of available mesh checking categories, use

the Select All or Deselect All buttons accordingly, or keep the default selection of all the items.

Domain Extents

Volume Statistics

Face Area Statistics

Number of Nodes per Edge

Number of Nodes per Face

Number of Nodes per Cell

Number of Faces/Neighbors per Cell

Cell Faces/Neighbors

Isolated Cells

Face Handedness

Periodic Face Pairs

Face Children

Zone Boundary Conditions

Invalid Node Coordinates

Poly Cells

. Once the cell zone(s) and the parameters are selected, click the Check button to perform the selective

mesh check, and view the output in the console window.The check is performed for the selected zone

and the corresponding adjacent faces, including the interiors of the selected zone, as well as any corres-

ponding edges.

You can perform a selective mesh check using the text user interface (TUI).

mesh/selective-mesh-check

The command will prompt you for one or more cell zones, as well as whether to include any of the

mesh check parameters. For example:

Meshing/mesh> selective-mesh-check

Select one or more cell zones for the mesh check.

Available cell zone(s): (solid_up: fluid1)

()

Cell Zones() [()] fluid1

Cell Zones() [()]

Specify selective mesh check parameters:

Domain Extents? [yes] y

Volume Statistics? [yes] y

Face Area Statistics? [no] n

Number of Nodes per Edge? [no] n

Number of Nodes per Face? [yes] n

Number of Nodes per Cell? [yes] n

Selectively Checking the Volume Mesh

Number of Faces/Neighbors per Cell? [no] n

Cell Faces/Neighbors? [no] n

Isolated Cells? [yes] n

Face Handedness? [yes] n

Periodic Face Pairs? [yes] n

Face Children? [yes] n

Zone Boundary Conditions? [yes] n

Invalid Node Coordinates? [yes] n

Poly Cells? [yes] n

Once the prompts are complete, the mesh check will proceed and display the results in the console

window. For example, given the previous input example, the output would look like:

Mesh check for cell zone(s): (fluid1)

x-coordinate: min = -.627150e+, max = .345894e+.

y-coordinate: min = -.250188e+, max = .475194e-.

z-coordinate: min = -.018144e+, max = .343869e+.

minimum volume: .420005e-.

maximum volume: .548519e+.

total volume: .211535e+.

Done.

It is important to check the quality of the volume mesh to evaluate whether it is sufficient for the

Done.

problem you are modeling. It is recommended that you check the mesh quality before transferring the

mesh data to solution mode or writing out the mesh/case file.

You can obtain information about the volume mesh quality by selecting the Mesh/Check Quality menu

item.

Mesh → Check Quality

When you select Mesh → Check Quality, the quality information will be printed in the console. The

sample output is as follows:

Mesh Quality:

Minimum Orthogonal Quality = .07960e-

(To improve Orthogonal quality, use "Inverse Orthogonal Quality",

where Inverse Orthogonal Quality =  - Orthogonal Quality)

Maximum Aspect Ratio = .42664e+

Note

The quality reported corresponds to that reported using the Report Quality button in the

General task page in solution mode (refer to Mesh Quality (p. ) for details).

For information about additional quality metrics, set the /mesh/check-quality-level to  prior

to using the Mesh → Check Quality option. In addition to the orthogonal quality and Fluent aspect

ratio, additional metrics such as cell squish and skewness will be reported when the check-quality-

level is set to .

If you are dissatisfied with the volume mesh generated, you can choose to clear the mesh and start

again from the boundary mesh. When the mesh is cleared, all interior nodes and faces, and all cells

both live and dead are deleted. Only the boundary nodes and faces will be left. After the mesh is cleared,

you can generate a new mesh.

This feature is available via Mesh → Clear.

You can also use the text command /mesh/clear-mesh. To delete the boundary mesh, use the text

command mesh/reset-mesh. When you use either of these commands you will be asked to confirm

that you want to clear or reset the mesh.

Important

If you have used domains to generate the mesh or grouped zones for reporting (as described

in Using Domains to Group and Mesh Boundary Faces (p. )), only the mesh in the active

domain will be cleared.

Clearing the Mesh

Chapter : Examining the Mesh

The following sections explain how to examine the mesh visually as well as manipulate the graphics

display and mouse function. You can specify various parameters that affect how the mesh appears in

the graphics window, manipulate the lighting and create composite views, control the display environ-

ment, modify the mouse button functions, and set program control variables.

.. Displaying the Mesh

.. Controlling Display Options

.. Modifying and Saving the View

.. Composing a Scene

.. Controlling the Mouse Buttons

.. Controlling the Mouse Probe Function

.. Annotating the Display

.. Setting Default Controls

You can manipulate the display of mesh entities and modify the way they appear in the graphics window.

Options exist for drawing and selecting the entities at your choice of complexity (object, zone, face,

edge, node). Tools exist for setting colors or highlighting based on specific parameters such as free or

multiply-connected, size field, or geometry recovery. You can also manipulate the display to show a

cross-section, adjust lighting, or overlay multiple images.

... Generating the Mesh Display using Onscreen Tools

... Generating the Mesh Display Using the Display Grid Dialog Box

The most commonly used mesh display tools are easily accessible in the graphical user interface ribbon.

For more flexibility and advanced display controls, see Generating the Mesh Display Using the Display

Grid Dialog Box (p. ).

In the Model tree, select the objects to be displayed using the right mouse button. At the global

Geometry Objects or Mesh Objects level, you can choose to Draw All. At the individual object level,

the Draw menu item allows you to draw the selected object exclusively, or use the Draw Options

menu to Add to or Remove from the existing display, as well as Highlight or Select the object.

In the meshing mode ribbon, there are groups of tools to interactively crop the display of the mesh,

to assist in selecting zones or objects, or to modify how the model is displayed in the graphics window.

You can use the Bounds group to limit the display to within a specified distance of a selected entity.

Select an entity (node, edge, face, zone) and specify a Delta value. The Set Ranges and Reset

buttons affect all directions simultaneously, or enable and disable the directions individually.

Enable Cutplanes to limit the graphics display to within delta value of the selected entity in

the selected ranges.

Tip

The settings in the Bounds group are also available when examining the volume

mesh. The Display → Grid dialog box has a Bounded check box on the Cells tab,

Tip

and the Cell Zones context menu includes an option to display the cells in the

specified range.

You can use the Clipping Planes group to interactively crop the display in one direction and pan the

cropped view as necessary.

Enable Insert Clipping Planes and use the slider to adjust the viewing limits. You can use the

Flip and Limit in options to further manipulate the position and direction of the clipping plane.

You can also use the Show Cut Edges option to display the cut edges of the model exposed

by the clipping plane. This option is disabled by default.

Enable the Draw Cell Layer option in order to quickly visualize a layer of cells of the volume

mesh on the clipping plane. Once the Draw Cell Layer option is enabled, you can enable the

Freeze Cell Layer option in order to keep the displayed cell layer in place as you continue to

study the mesh using other tools.

To draw a layer of cells on the clipping plane for specific cell zones, select the cell zone(s) under

Mesh Objects in the Tree and use the Draw Cell Layer option in the context menu.

You can use the Selection Helper group to assist in selecting zones or objects by a Name Pattern

(wild cards accepted) and Geometry Recovery level.

Use the Filter drop down to specify face zones, edge zones, objects, object face zones or object

edge zones for selection. The Advanced button opens a dialog box offering more options for

zone selection.

You can use the Selection group to choose how to select entities using the mouse in the graphics

display.

display.

The Global Display group contains several check boxes to enable or disable certain elements of the

graphics window (Title, Help Text) or model display (Faces, Edges, Highlights).

The Local Display group contains several tools to help with visualizing the current model.These include

Transparency, Exploded view, Centroid, Edge Zone selection mode, Face edge display and Measure

Distance.

Several on-screen tool buttons have associated hot-keys. A complete list is available in Shortcut Key

Actions (p. ).

The Display Grid dialog box includes a full set of tools to control the display of items using several

criteria.

Examining the Mesh

To generate the mesh display:

.

Select Display → Grid....

.

Select the entities to be displayed in the Zones lists in the Nodes, Edges, Faces, or Cells tabs.You can

also select several entities of the same group using the Zone Groups lists in these tabs.

.

Select the display Options as appropriate from the group box in the Nodes, Edges, Faces, or Cells tabs.

You may select intrinsic parameters such as skewness or size. When you specify a range for a

particular parameter, the entities that satisfy that condition are displayed. If more than one range

limitation is specified, then only those entities that match all specified range limitations are drawn.

.

The Bounds tab offers enhanced functionality relative to the ribbon group.

You may insert up to six cutplanes (two in each of the x-, y-, and z-direction) and asymmetrically

control their location based on specific coordinates. Alternatively, you can compute ranges based

on the proximity to a selected entity.

.

Set the display options as appropriate in the Attributes tab. See Mesh Display Attributes (p. )

You can specify information regarding color, display of solid (filled) faces, and shrinkage of faces

and cells. These features can help you visualize your mesh effectively and quickly determine the

cause of any problems in the mesh.

.

Click Display to draw the mesh in the active graphics window.

To cancel a display operation, press Ctrl+C while the data is being processed in preparation for

graphical display. You cannot cancel the operation after the program begins to draw in the

.... Mesh Display Attributes

The mesh display options include modifying the mesh colors, adding the outline of important features

to a display, displaying normals, shrinking the faces and/or cells in the display, adding lights for filled

mesh displays, and so on.

Modifying the Mesh Colors

You can control the colors used to render the mesh for each zone type or entity. You can modify the

colors using the Grid Colors dialog box.

.

To open the Grid Colors dialog box, go to the Attributes tab in the Display Grid dialog box, and click

Colors....

By default, the Color by Type option is selected, enabling you to assign colors based on zone

type.

.

To change the color assigned to a particular zone type, select the zone type in the Types list.

.

Select the required color in the Colors list.

.

If you prefer to assign colors based on the zone ID, select the Color by ID option.

Displaying the Mesh

.

.

.

.

Select Color by Normal to color one side of the faces in grey and the other side in yellow, depending

on the normal direction.The side colored grey indicates normal direction (normals pointing toward

you), while the side colored yellow has normals pointing away.

Important

You can set colors individually for the mesh displayed on each of the zones using the

Scene Description dialog box.

Adding Features to an Outline Display

For closed 3D geometries, the standard outline display may not show sufficient details to accurately

depict the shape. This is because for each boundary, only the edges on the outside of the geometry

(that is, those used by only one face on the boundary) are drawn. You can capture additional features

using the Feature option in the Display Grid dialog box. Specify an appropriate value for the Feature

Angle to obtain the outline display required.

Shrinking Faces and Cells in the Display

To distinguish individual faces or cells in the display, you may want to enlarge the space between

adjacent faces or cells by increasing the Shrink Factor in the Display Grid dialog box. The default

value of zero produces a display in which the adjacent faces or cells overlap. A value of  creates the

opposite extreme, where each face or cell is represented by a point and there is a considerable space

between entities. A small value such as . may be sufficient to enable you to distinguish a face or

cell from its neighbor. Figure . : Mesh Display (A) With Shrink Factor =  (B) With Shrink Factor =

. (p. ) shows displays with different Shrink Factor values.

Figure . : Mesh Display (A) With Shrink Factor =  (B) With Shrink Factor = .

Adding Lights

You can add lights with a specified color and direction to your display. These lights can enhance the

appearance of the display, especially for 3D geometries.

To enable the effect of lighting using the Display Options dialog box, enable Lights On in the Lighting

Attributes group box and click Apply.You can also choose the method to be used in lighting interpolation.

Select Flat, Gouraud, or Phong in the Lighting drop-down list. Flat is the most basic method: there is

no interpolation within the individual polygonal facets. Gouraud and Phong have smoother gradations

of color because they interpolate on each facet.

The Lights dialog box contains options for creating lights and then enabling/disabling individual lights

as needed. In this way, you can retain lights that you have defined previously but do not want to use at

present.

The default light, light  is defined to be dark gray with a direction of (,,). To define additional

lights, do the following:

.

Increase Light ID to a new value (for example, ).

.

Enable Light On.

.

Define the light color by entering a descriptive string (for example, lavender) in the Color field, or

by moving the Red, Green, and Blue sliders to obtain the desired color.The default color for all lights

is dark gray.

.

Specify the light direction by doing one of the following:

– Enter the (X,Y, Z) Cartesian components under Direction.

– Click the middle mouse button in the desired location on the sphere under Active Lights. (You

can also move the light along the circles on the surface of the sphere by dragging the mouse while

holding down the middle button.) You can rotate the sphere by pressing the left mouse button

and moving the mouse (like a trackball).

– Use your mouse to change the view in the graphics window so that your position in reference to

the geometry is the position from which you would like a light to shine.Then click Use View Vector

to update the X,Y,Z fields with the appropriate values for your current position and update the

graphics display with the new light direction.This method is convenient if you know where you

want a light to be, but you are not sure of the exact direction vector.

.

Repeat steps – to add more lights.

.

When the lights have been defined, click Apply in the Lights dialog box to save the definitions.

To remove a light, enter the ID number of the light to be removed in the Light ID field and then

clear the Light On check box. When a light is disabled, its definition is retained, so you can easily

add it to the display again at a later time by selecting the Light On check box.

If you have made changes to the light definitions, but you have not yet clicked Apply, you can

reset the lights by clicking Reset. All lighting characteristics will revert to the last saved state (that

is, the lighting that was in effect the last time you opened the dialog box or clicked on Apply).

Using Styles

The Style Attributes dialog box is opened by clicking on the Styles... button in the Attributes tab

frame of the Display Grid dialog box. It controls the appearance of faces, edges, and nodes that are

displayed using the Display Grid dialog box. To modify the attributes of a certain type of face, edge,

or node (e.g., unmeshed), select the appropriate item in the Styles list, change the parameters, and

click Apply. You will see the effect of these changes the next time you display the grid.

Table . : Default Style Attributes

Size

Symbol

Color

Visible

Weight

Color

Nodes

Visible

Edges

Color

Faces

Visible

Styles

.

o

red

yes

red

yes

red

yes

left-handed

.

magenta o

yes

yellow

yes

magenta

yes

refine

.

o

orange

yes

foreground2

yes

cyan

yes

free

.

magenta o

yes

yes

yellow

yes

multi

.

o

red

yes

orange

yes

–

no

unmeshed

.

x

green

yes

green

yes

–

no

unused

.

magenta o

yes

yellow

yes

magenta

yes

mark

.

magenta o

yes

yellow

yes

magenta

yes

tag

–

–

–

no

foreground1

yes

blue

yes

face-size

–

–

–

no

red

yes

–

no

cell-size

–

–

–

no

yes

red

yes

face-quality

–

–

–

no

red

yes

–

no

cell-quality

The Display Options dialog box contains options for changing some of the rendering parameters for

the mesh displayed in the graphics window. You can also control the lighting attributes in a scene or

modify parameters based on the graphics hardware and software you are using or change the graphics

window layout or color scheme. After making a change to any of the parameters, click Apply to update

the active graphics window with the new attributes.

Display → Options...

Rendering

The following Rendering options are available:

Line Width

Rendering

Line Width

Use this control to increase the width from the default value of  pixel.

Point Symbol

The default symbol is a + sign inside a circle. Selecting a different symbol in the Point Symbol drop-down

list may help visibility in some situations.

Animation Options

There are two animation options that you can choose from:

All

uses a solid-tone shading representation of all geometry during mouse manipulation.

Wireframe

uses a wireframe representation of all geometry during mouse manipulation. If your computer has a

graphics accelerator, you may not want to use this option; otherwise, the mouse manipulation may

be very slow.

Double Buffering

Enabling the Double Buffering option can dramatically reduce screen flicker during graphics updates.

Note, however, that if your display hardware does not support double buffering and you turn this option

on, double buffering will be done in software. Software double buffering uses extra memory.

Outer Face Culling

This option enables you to turn off the display of outward pointing faces of shells or meshes.This is

sometimes useful for displaying both sides of a slit wall. By default, when you display a slit wall, one side

will “bleed” through to the other.When you enable the Outer Face Culling option, the display of a slit

wall will show each side distinctly as you rotate the display.This option can also be useful for displaying

two-sided walls (that is, walls with fluid or solid cells on both sides). Please note, however, that enabling

it can also hides some unintended surfaces on certain viewing angles, e.g. while displaying Contours, it

might be visible only from one side of the surface and not from the other

Hidden Surface Removal

If you use hidden surface removal, ANSYS Fluent will try to determine which surfaces in the display are

behind others. If you do not use hidden surface removal, all surfaces will be displayed, and a cluttered

display will result for most 3D mesh displays.

You can choose one of the following methods for performing hidden surface removal in the Hidden

Surface Method drop-down list. These options vary in speed and quality, depending on the device

you are using.

Hardware Z-buffer

is the fastest method if supported by your hardware.The accuracy and speed of this method is hardware

dependent.

Painters

will show fewer edge-aliasing effects than hardware-z-buffer.This method is often used instead of

software-z-buffer when memory is limited.

Software Z-buffer

is the fastest of the accurate software methods available (especially for complex scenes), but it is

memory intensive.

Z-sort only

is a fast software method, but it is not as accurate as software-z-buffer.

Color Scheme

Choose the background color — gradient (Workbench) or solid black (Classic).

Layout

Choose to enable or disable additional display status information:

Controlling Display Options

Titles: caption block area below the graphic containing date, product, and contents of the display.The

caption block supports limited text editing. Position the cursor at the end of a line to add or delete text.

Text in the caption block will not be deleted when you clear Annotations.

Axes: X-Y-Z triad showing orientation. Click on the tip of one axis to rotate the model to the selected ortho-

gonal view, or the cyan-colored dot for isometric view.

Scale Ruler:Visual indicator showing the size in the plane of the graphics display.The indicator automatically

resizes as the model is zoomed in the graphics display.

Logo: ANSYS and version number.

Colormap: when displaying simulation results, the scale may be shown as function of the visible spectrum.

Graphics Device Information

If you need to know which graphics driver you are using and what graphics hardware it recognizes,

you can click Info in the Display Options  dialog box. The graphics device information will be printed

in the text window.

Note

When working remotely, you can optimize the graphics window settings using the text

command remote-display-defaults. Restore the settings for your local display

using the text command native-display-defaults.

You can use the Views dialog box to control the model orientation and zoom level in the graphics

window.

Display → Views

You can choose isometric or one of the standard orthographic views from the list.The displayed model

will be centered and zoomed to fit the available graphics window.

You can also use the Set view shortcut (

) in the View Tools (p. ) to set one of the

standard views.

You can modify the view by scaling, centering, or rotating the model.You can Save a modified view

or Delete any view from the list.

You can use Write... to open the Write Views dialog box to save selected views to a file, which you

can Read... and use with other mesh files.

... Mirroring a Non-symmetric Domain

You can use the Mirror Planes dialog box to define a symmetry plane for a non-symmetric domain

for use with graphics. Click Define Plane... to open the dialog box.

.

In the Plane Equation group box, specify the coefficients of A, B, C, and the distance from the origin.

The equation for the mirror plane will be Ax+By+Cz=distance.

.

Click Add.

The Mirror Planes list contains a list of all mirror planes you have defined (but not the mirror

planes that exist in the domain due to symmetry as they cannot be modified).

.

Select a mirror plane from the list. Click Apply to see both the original and the mirrored image in the

... Controlling Perspective and Camera Parameters

You can use the Camera Parameters dialog box to control perspective and modify the “camera”

through which you are viewing the graphics display instead of translating, rotating, and zooming the

display.

You can choose to display a perspective view of the graphics (default) or an orthographic view. Select

the appropriate option in the Projection drop-down list in the Camera Parameters dialog box..

The Camera is defined by four parameters (see Figure . : Camera Definition (p. )):

Figure . : Camera Definition

Position is the camera’s location.

Target  is the location of the point the camera is looking at.

Up Vector indicates to the camera which way is up.

Field indicates the field of view (width and height) of the display.

Modifying and Saving the View

Select the parameter to be modified and specify the coordinates or field distances in the X, Y, and Z

fields. Click Apply after you change each camera parameter.

Important

When using the sliders and dial to manipulate the view, select All in the Display Options

dialog box so that you can watch the display move interactively while you move the slider

or the dial indicator.

After displaying the mesh or parts of the mesh in your graphics window, you may want to overlay an

additional display or move entities around and change their characteristics to increase the effectiveness

of the scene displayed.

Display → Scene...

You can use the Scene Description dialog box—and the Display Properties dialog box and the

Transformations dialog box that are opened from it—to rotate, translate, and scale each entity indi-

vidually, as well as to change the color and visibility of each entity. You can make geometric entities

visible and invisible, thereby adding or deleting entities from the scene one at a time.

... Changing the Display Properties

...Transforming Geometric Entities in a Scene

... Adding a Bounding Frame

... Using the Scene Description Dialog Box

To enhance the scene in the graphics window, you can change the color, visibility, and other display

properties of each geometric entity in the scene using the options available in the Display Properties

You can specify different colors for displaying the edges and faces of a zone to show the underlying mesh

(edges) when the faces are filled and shaded.

You can also make a selected entity temporarily invisible. If, for example, you are displaying the entire mesh

for a complicated problem, you can make entities visible or invisible to display only certain boundary zones

of the grid without regenerating the grid display using the Display Grid dialog box.

You can also use the visibility controls to manipulate geometric entities for efficient graphics display.

For details, refer to Using the Scene Description Dialog Box (p. ).

When composing a scene in your graphics window, it is helpful to move a particular entity from its

original position or to increase or decrease its size. For example, you may want to temporarily move

an interior portion of the mesh outside the mesh boundaries where it can be seen and interpreted

more easily.

You can also move an entity by rotating it about a specified point. If you want to display one entity

more prominently than the others, you can scale its size. All these capabilities are available in the

Transformations dialog box.

You can optionally add a bounding frame to the display of the domain and include measure markings

to indicate the length, height, and/or width of the domain using the Bounding Frame dialog box.

Figure . : Graphics Display with Bounding Frame

To add a bounding frame to the display:

.

Click Frame Options... in the Scene Description dialog box.

.

Select Domain or Display in the Frame Extents list to indicate whether the bounding frame should

encompass the domain extents or only the portion of the domain that is shown in the display.

.

.

.

Indicate the bounding plane(s) to be displayed by clicking on the white square on the appropriate plane

of the box shown under the Axes heading.You can use any of the mouse buttons.The square will turn

red to indicate that the associated bounding plane will be displayed in the graphics window.

.

Specify where you would like to see the measurement annotations by clicking on the appropriate edge

of the box.The edge will turn red to indicate that the markings will be displayed along that edge of the

displayed geometry

.

Click Display to update the display with the current settings.

If you want to include the bounding frame in all subsequent displays, enable the Draw Frame option

in the Scene Description Dialog Box and click Apply. If this option is not enabled, the bounding box

will appear only in the current display; it will not be redisplayed when you generate a new display

(unless you have overlays enabled).

You can use the Scene Description dialog box and its associated dialog boxes as follows:

.

Select the mesh entities in the Names selection list in the Scene Description dialog box.

Composing a Scene

The Names list is a list of the mesh entities that currently exist in the scene (including those that

are presently invisible). If you select more than one entity, any operation (color specification,

transformation, and so on) will apply to all the selected entities. You can also select the entities

by clicking them in the graphics window using the mouse probe button (right mouse button, by

default).

.

default).

.

Set the color, visibility, and other display properties for the mesh entities selected using the Display

Properties dialog box.

You can specify different colors for individual mesh entities.You can specify different colors for dis-

playing the edges and faces of a zone to show the underlying mesh (edges) when the faces of the

grid are filled and shaded.

To modify the color of faces, edges, or lines, choose face-color, edge-color, line-color, or node-

color in the Color drop-down list. The Red, Green, and Blue color scales will show the RGB

components of the face, edge or line color, which you can modify by moving the sliders on the

color scales. When you are satisfied with the color specification, click Apply to save it and update

the display.

You can control the visibility of individual mesh entities using the Visible option. Hence, you can make

an entity visible or invisible to display only certain boundary zones, without regenerating the entire

mesh display.

To enable the effect of lighting for the selected entities on or off, select Lighting.You can choose to

have lighting affect only certain entities instead of all of them.

To toggle the filled display of faces for the selected zones, use the Faces option. Enabling Faces on

here has the same effect as turning it on for the entire mesh in the Display Grid dialog box.

To enable the display of outer edges, use the Outer Faces option.This option is useful for displaying

both sides of a slit wall. By default, when you display a slit wall, one side will “bleed” through to the

other.When you disable the Outer Faces option, the display of a slit wall will show each side distinctly

as you rotate the display.This option can also be useful for displaying two-sided walls (that is, walls

with fluid or solid cells on both sides).

To enable/disable the display of interior and exterior edges of the zones, select Edges.

To enable/disable the display of the outline of the zones, select Perimeter Edges.

To enable/disable the display of feature lines, select Feature Edges.

To enable/disable the display of the lines, select Lines.

To enable/disable the display of nodes, select Nodes.

.

To overlay one display over another, select the mesh entities in the Names selection list, enable Overlays

in the Scene Composition group box and click Apply. Once overlaying is enabled, subsequent graphics

that you generate will be displayed on top of the existing display in the active graphics window.To

generate a plot without overlays, you must disable the Overlays option and click Apply.

Note

To overlay bounded cell zones over face zones in the display, do the following:

.

Display only the bounded cell zones (face zones should not be selected).

.

Select the cell zones in the Names selection list in the Scene Description dialog box,

enable Overlays and click Apply.

.

Display the face zones with the appropriate bounds specified.

If you select the bounded face zones first and enable Overlays, you will need to deselect

the face zones in the Display Grid dialog box before displaying the bounded cell zones.

.

To transform the entities displayed, select the mesh entities in the Names selection list in the Scene

Description dialog box and click Transform... to open the Transformations dialog box for the selected

entities.

entities.

To translate the selected entities, enter the translation distance in each direction in the X,Y, and Z real

number fields under Translate.

To rotate the selected entities, enter the number of degrees by which to rotate about each axis in the

X,Y, and Z integer number fields under Rotate By.You can enter any value between - and .

By default, the rotation origin will be (,,). If you want to spin an entity about its own origin, or about

some other point, specify the X,Y, and Z coordinates of that point under Rotate About.

To scale the selected entities, enter the amount by which to scale in each direction in the X,Y, and Z

real number fields under Scale.To avoid distortion of the shape, be sure to specify the same value for

all three entries.

You can assign a specific function to each of the mouse buttons using the Mouse Buttons dialog box.

These functions apply only to the graphics windows; clicking a mouse button in the graphics window

will cause the appropriate action to be taken.

Display → Mouse Buttons...

Important

3DConnexion Space products (Ball, Mouse, Pilot, and Navigator) are not supported with

Fluent.

The predefined button functions available are as follows:

mouse-rotate

enables you to rotate the view by dragging the mouse across the screen.

Horizontal mouse movement rotates the entity about the screen’s y-axis.

Vertical mouse movement rotates the entity about the screen’s x-axis.

The function completes when the mouse button is released or the cursor leaves the graphics window.

Controlling the Mouse Buttons

mouse-dolly

enables you to translate the view by dragging the mouse while holding down the button.The function

completes when the mouse button is released or the cursor leaves the graphics window.

mouse-zoom

enables you to draw a zoom box, anchored at the point at which the button is pressed, by dragging the

mouse.When you release the button:

If the dragging was from left to right, a magnified view of the area within the zoom box will fill the

window.

If the dragging was from right to left, the area of the window shrinks to fit into the zoom box, resulting

in a “zoomed out” view.

If the mouse button is clicked (not dragged), the selected point becomes the center of the window.

mouse-roll-zoom

enables you to zoom in or out, or rotate the model, by rolling the mouse while the button is pressed.

If dragging up or down, the image is zoomed out or in, respectively.

If dragging left or right, the image is rotated about the screen’s z-axis.

mouse-probe

enables you to perform the specified mouse probe function.The mouse probe function can be set in the

Mouse Probe dialog box (see Controlling the Mouse Probe Function (p. )).

mouse-annotate

enables you to insert text into the graphics window. If you drag the mouse, an attachment line is drawn.

When you release the button, a cursor displays in the graphics window and you can enter the text. Press

Enter or move the cursor out of the graphics window.

To remove annotated text and attachment lines, select Clear button in the Annotate dialog box.

This deletes all annotated text from the window.

You can assign a specific mouse probe function and filter using the Mouse Probe dialog box. Once set,

clicking the mouse probe button in the graphics window causes the action to occur.

Display → Mouse Probe...

Use the Function list to choose an action for the mouse probe button.

off

disables the mouse probe.

label

displays the label for the selected entity in the graphics window.

select

enables the selection of an entity by clicking.The selected entity is highlighted in the graphics window

and, if open, in a list in most dialog boxes.

print

prints information about the selected entity in the console. See Reporting Mesh Information (p. ) for a

description of the output.

box

enables the selection of a group of entities within a box.The selected entities are highlighted in the

graphics window and, if open, in a list in most dialog boxes.To define the selection box, click the mouse

probe button at one corner of the region to be selected, drag the mouse to the opposite corner, and release

the mouse probe button.

polygon

enables the selection of a group of entities within a polygonal region.The selected entities are highlighted

in the graphics window and, if open, in a list in most dialog boxes.To define the selection polygon, click

the mouse probe button at one vertex of the polygonal region to be selected, and use the left mouse

button to successively select each of the remaining vertices.

Click the mouse probe button again (anywhere in the graphics window) to complete the polygon

definition.

Use the Filter selection list to specify the type of entity selected. The available filters are off, cell, face,

edge, node, zone, position, object, and size.

Note

If off is chosen and a selection is made, it is first checked to see if it is a cell, then a face, an edge,

and so on.

When the node filter is used, if a cell or face is selected the node closest to the selection point

is picked.Thus nodes do not have to be displayed to be picked.

When using box select or polygon select, by default, all entities will be selected. To select only visible

entities (nodes, faces, zones, objects) instead, enable Select Visible Entities in the Mouse Probe

Function group in the ribbon. The selection will then include only entities visible to the eye, and not

those hidden behind other entities in the display. When enabled, ensure that the model is zoomed to

an appropriate level for correct selection.

Note

If the mesh is not connected, all entities (nodes, edges, faces, zones, objects) will be selected

This visual selection behavior works only on local displays and may generate warning mes-

sages when attempting selection on a remote system.

Text annotations with optional attachment lines may be added to the graphics windows.

Display → Annotate...

Annotating the Display

The text is added to the window at a location chosen with the mouse, using the mouse-probe button

(see Controlling the Mouse Buttons (p. ) for information on setting the mouse buttons). Dragging

with the mouse-probe button pressed will draw an attachment line from the point where the mouse

was first clicked to the point where it was released. The annotation text will be placed at the point

where the mouse button was released.

The annotation text is associated with the active graphics window; it is removed only when the annota-

tions are explicitly cleared. You can edit the text in the graphics window’s caption block by the left

mouse button in the desired location. When a cursor appears, you can type the new text or delete the

existing text. Text in the caption block will not be deleted when you clear annotations.

The Display → Controls menu item opens the Controls dialog box to set file-specific variables called

tgvars.

The dialog box has two components: the Categories drop-down list and the actual variables associated

with that category.

Select the desired category, and then enter the desired default values. Click Apply to update your file

with the new values.

Chapter : Determining Mesh Statistics and Quality

The best way to determine the quality of a mesh is by looking at statistics such as maximum skewness,

rather than just performing a visual inspection. Unlike structured meshes, unstructured meshes are

nearly impossible to comprehend with only a graphical plot. The Report menu has a variety of reporting

capabilities. The types of mesh information that can be reported include:

The size of the mesh (that is, the number of nodes, faces, and cells in it): use the Report Mesh Size dialog

box.

box.

Report → Mesh Size...

Minimum, maximum, and average values of face size and quality: use the Report Face Limits dialog box.

Report → Face Limits...

Minimum, maximum, and average values of cell size and quality in a volume mesh: use the Report Cell

Limits dialog box.The default quality measure is skewness, but you can also report the limits based on

other quality measures or the range of change in cell size.

Report → Cell Limits...

Boundary cell quality limits: use the Report Boundary Cell Limits dialog box.

Report → Boundary Cell Limits...

Information about individual components of the mesh: use the print-info command.

Important

If you used domains to generate the mesh or group zones for reporting (as described in

Using Domains to Group and Mesh Boundary Faces (p. )), the report will apply only to the

active domain.

These reporting operations are described in the following sections.

.. Determining Mesh Statistics

.. Determining Mesh Quality

.. Reporting Mesh Information

The Report Mesh Size dialog box reports the number of nodes, faces, and cells. Nodes and faces are

grouped into those defining the boundaries and those used inside cell zones. Click Update to view the

latest mesh statistics.

If the generation of the initial mesh fails, you can determine the number of meshed boundary nodes

and faces by enabling Report Number Meshed in the Report Mesh Size dialog box. The headings Bound-

ary and Interior will be replaced by Total and Meshed, respectively, and the total number of boundary

nodes and faces will be reported along with the number that were meshed.

A good quality mesh guarantees the best analysis results for the problem, minimizes the need for addi-

tional analysis runs, and improves your predictive capabilities. The mesh should be fine enough to resolve

the primary features of the problem being analyzed. The mesh resolution  depends on the boundary

mesh from which you start and the parameters controlling the generation of the interior mesh. In a

high-quality mesh, the change in size from one face or cell to the next should be minimized. Large

differences in size between adjacent faces or cells will result in a poor computational mesh because

the differential equations being solved assume that the cells shrink or grow smoothly.

... Determining Surface Mesh Quality

... Determining Volume Mesh Quality

... Determining Boundary Cell Quality

... Quality Measure

Before generating a volume mesh, check the quality of the faces to get an indication of the overall

mesh quality. To check face size and quality limits, use the Report > Face Limits... dialog box. For 3D

meshes, a maximum of less than . and an average of . are good. The lower the maximum skewness,

the better the mesh. See Quality Measure (p. ) for information on face and cell quality measures

The default quality measure is skewness, but you can also report other quality measures such as the

aspect ratio limits or the range in size change for a face zone. Before creating a layer of pyramid cells,

check the aspect ratio of the quadrilateral faces that will form the base of the pyramids. This aspect

ratio should be less than , otherwise the triangular faces of the pyramids will be highly skewed. If the

aspect ratio is greater than , regenerate the quadrilateral faces:

If the quadrilateral faces were created in a different preprocessor, return to that application and try to reduce

the aspect ratio of the faces in question.

If the quadrilateral faces were created during the building of prism layers, rebuild the prisms using a more

gradual growth rate.

Check the skewness of triangular faces on a boundary from which you are going to build prisms to

ensure that the quality of the prism cells will be good. After you create the prisms, check the skewness

of the triangular faces that were created during the prism generation.

Face Distribution histogram

When checking the quality of the mesh you may find it useful to look at a histogram of boundary face

quality or size. You can generate such a plot or report using the Face Distribution dialog box.

Display → Plot → Face Distribution

The number of faces on the selected zones with a size or quality measure value (e.g., skewness) in the

axis shows the size or quality and the y axis gives the number of faces or the percentage of the total

number of faces.

Determining Mesh Statistics and Quality

You can modify the appearance of the histogram using the options available in the Axes dialog box.

The following parameters can be modified:

Labels for the axes.

Scaling of the axes: decimal (default) or logarithmic.

Range of values: enable Auto Range or specify minimum and maximum values.

Major and minor rules: horizontal or vertical lines marking the primary and secondary data divisions,

respectively.You can select the line color and thickness to be used.

Number format.

You can also modify the appearance of the histogram using the options available in the Curves dialog

box. The following parameters can be modified:

Line style patterns, colors, and weight.

Marker symbols, colors, and styles.

When the histogram plot is displayed in the graphics window, you can use any of the mouse buttons

to add text annotations to the plot. See Controlling the Mouse Buttons (p. ) and Annotating the

Display (p. ) for more information about using the mouse buttons and annotation features.

After generating the volume mesh, check the quality of the cells to get an indication of overall mesh

quality. The quality of the mesh plays a significant role in the accuracy and stability of the numerical

computation. To check cell size and quality limits, use the Report > Cell Limits... dialog box.

aspect ratio limits or the range in size change for a cell zone. See Quality Measure (p. ) for information

on face and cell quality measures available.

Cell Distribution histogram

You can generate a histogram plot to graphically display cell size or quality by using the controls in

the Cell Distribution dialog box.

Display → Plot → Cell Distribution

The number of cells in the selected zones with a size or quality value (e.g., skewness) in the specified

range in each of the regularly spaced partitions is displayed in a histogram format. The x axis shows

either the size or the quality and the y axis gives the number of cells or the percentage of the total.

Determining Mesh Quality

to add text annotations to the plot. For more information about the annotation features, see Controlling

the Mouse Buttons (p. ) and Annotating the Display (p. ).

For boundary layer flows, boundary cells with low skewness are very important. Use the Report

Boundary Cell Limits dialog box to report the quality of cells containing a specified number of

boundary faces or nodes.

For tetrahedral meshes, the maximum skewness will not be lower than the maximum face skewness,

because the boundary cell skewness is limited by the boundary face skewness.

You can remove highly skewed cells with two boundary faces by using the Tet Improve dialog box.

Mesh → Tools → Tet Improve...

To specify the quality measure (skewness, aspect ratio, change in size, and so on), use the Quality

Measure dialog box. The default quality measure is skewness.

Report → Quality Measure...

Mesh quality is determined by the following quality measures:

Skewness

Skewness is one of the primary quality measures for a mesh. Skewness determines how close to ideal

(that is, equilateral or equiangular) a face or cell is:

Figure . : Ideal and Skewed Triangles and Quadrilaterals

The following table lists the range of skewness values and the corresponding cell quality.

Table . : Skewness Ranges and Cell Quality

Cell Quality

Skewness

degenerate

bad (sliver)

.–<

poor

.–.

fair

.–.

good

.–.

excellent

>–.

equilateral

According to the definition of skewness, a value of  indicates an equilateral cell (best quality) and

a value of  indicates a completely degenerate cell. Degenerate cells (slivers) are characterized by

nodes that are nearly coplanar. Cells with a skewness value above  are invalid.

Highly skewed faces and cells should be avoided because they can lead to less accurate results

than when relatively equilateral/equiangular faces and cells are used.

Two methods for measuring skewness are:

Based on the equilateral volume (applies only to tetrahedra).

Based on the deviation from a normalized equilateral angle.This method applies to all cell and face

shapes, such as pyramids and prisms.

The default skewness method for tetrahedra is the equilateral volume method, but you can change

to the angle deviation method using the Quality Measure dialog box.

Equilateral-Volume-Based Skewness

In the equilateral volume deviation method, skewness is defined as

(.)

where, the optimal cell size is the size of an equilateral cell with the same circumradius.

In 3D meshes, most cells should be rated good or better, but a small percentage will generally be

in the fair range and there are usually even a few poor cells. The presence of poor cells can indicate

poor boundary node placement. You should try to improve your boundary mesh as much as possible

because the quality of the overall mesh can be no better than that of the boundary mesh.

Normalized Equiangular Skewness

In the normalized angle deviation method, skewness is defined (in general) as

(.)

where

= largest angle in the face or cell

= smallest angle in the face or cell

= angle for an equiangular face/cell (such as  for a triangle,  for a quad, and so on)

The cell skewness will be the maximum skewness computed for any face. For example, an ideal

pyramid (skewness = ) is one in which the  triangular faces are equilateral (and equiangular) and

the quadrilateral base face is a square. The guidelines in Table . : Skewness Ranges and Cell

Quality (p. ) apply to the normalized equiangular skewness as well.

Size change is the ratio of the area (or volume) of a face (or cell) in the geometry to the area (or volume)

of each neighboring face (or cell).This ratio is calculated for every face (or cell) in the domain.The minimum

and maximum values are reported for the selected zones.

Edge Ratio

The edge ratio is defined as the ratio of maximum length of the edge of the element to the minimum

length of the edge of the element.

By definition, edge ratio is always greater than or equal to . The higher the value of the edge ratio,

the less regularly shaped is its associated element. For equilateral element shapes, the edge ratio

is always equal to .

The aspect ratio of a face or cell is the ratio of the longest edge length to the shortest edge length.The

aspect ratio applies to triangular, tetrahedral, quadrilateral, and hexahedral elements and is defined dif-

ferently for each element type.

The aspect ratio can also be used to determine how close to ideal a face or cell is.

For an equilateral face or cell (such as an equilateral triangle, a square, and so on), the aspect ratio is

.

For less regularly-shaped faces or cells, the aspect ratio will be greater than  as the edges differ in

length.

For triangular faces and tetrahedral cells and for pyramids, you can usually focus on improving the

skewness, and the smoothness and aspect ratio will consequently be improved as well.

For prisms, it is important to check the aspect ratio and/or the change in size in addition to the skewness,

because it is possible to have a large jump in cell size between two cells with low skewness or a high-

aspect-ratio low-skew cell.

Squish

Squish is a measure used to quantify the non-orthogonality of a cell with respect to its faces. It is defined

(.)

where

A = face unit area vector

= the vector connecting the adjacent cell centroids (for face squish) or the cell and face centroids

(for cell squish)

Warp (Quadrilateral Elements only)

Face warp applies only to quadrilateral elements and is defined as the variation of normals between the

two triangular faces that can be constructed from the quadrilateral face.The actual value is the maximum

of the two possible ways triangles can be created.

Mathematically, it is expressed as follows:

(.)

where

= the deviation from a best-fit plane that contains the element

,

= the lengths of the line segments that bisect the edges of the element

The value of face warp ranges between  and . A value of  specifies an equilateral element and

a value of  specifies a highly skewed element.

Dihedral angle applies only to faces and not cells.The dihedral angle is defined as the angle between the

normals of adjacent faces.This quality measure is useful in locating sharp corners in complicated geomet-

ries.The dihedral angle value ranges from –.

ICEM CFD Quality

The ICEM CFD quality measure calculates element quality based on the quality values in ANSYS

ICEM CFD. This measure is only available for cells, not faces.

Tetrahedra:The quality is calculated as the skewness of the tetrahedral element.

The remaining quality values are based on various quality metrics computed in ANSYS ICEM

CFD.

Quality =  - ANSYS ICEM CFD Quality

Hexahedra:The quality is based on the Determinant, Max Orthogls, and Max Warpgls metrics in ANSYS

ICEM CFD.

– The determinant is the ratio of the smallest and the largest determinant of the Jacobian matrices,

where a Jacobian matrix is computed at each node of the element.

– The max orthogls metric calculates the maximum deviation of the internal angles of the element

from  degrees. Angles between  and  degrees (deviation up to  degrees) will also be

considered.

– The warp for each face is calculated as the maximum angle between the triangles connected at the

diagonals of the face.The max warpgls metric is calculated as the maximum warp of the faces com-

prising the element.

These values are normalized and the minimum value of the three normalized diagnostics will

be used.

Pyramids:The quality is based on the Determinant computed in ANSYS ICEM CFD.

The determinant is the ratio of the smallest and the largest determinant of the Jacobian matrices,

Prisms:The quality is based on the Determinant and Warp computed in ANSYS ICEM CFD.

– The warp for each face is calculated as the maximum angle between the respective edges and a

plane containing the mid-points of the edges comprising the face.The warp for the element is then

calculated as the maximum warp of the faces comprising the element.

The quality is calculated as the minimum of the determinant and warp.

For further details on the quality measures available in ANSYS ICEM CFD, refer to the ANSYS ICEM

CFD Help Manual.

The range of quality values reported is between - (the range in ANSYS ICEM CFD is - to , and

a value of  corresponds to - in ANSYS ICEM CFD,  to , and  to , respectively). A value of

indicates a perfect, non-distorted element,  indicates a degenerate element, and values above

indicate an invalid element (such as concave, dihedral angle >  degree, or negative volume

elements).

Ortho Skew

The ortho skew quality for a cell is computed using the face normal vector,

for each face; the vector

from the cell centroid to the centroid of each of the adjacent cells,

; and the vector from the cell centroid

to the centroid of each face,

. Figure . :Vectors Used to Compute Ortho Skew/Inverse Orthogonal

Quality for a Cell (p. ) illustrates the vectors used to determine the ortho skew quality for a cell.

Figure . : Vectors Used to Compute Ortho Skew/Inverse Orthogonal Quality for a Cell

For each face , the calculation first finds the value of ( - the cosine of the angle between the face

normal vector and the corresponding vector from the centroid of the cell to the centroid of that

face):

(.)

Next, for each face , the calculation finds the value of ( - the cosine of the angle between the

face):

(.)

face normal vector and the corresponding vector from the centroid of the cell to the centroid of

the adjacent cell that shares that face):

(.)

The reported Ortho Skew quality for a cell then depends on the cell type:

For most cells, Ortho Skew is the maximum of the above quantities computed for each face.

For pyramid cells, Ortho Skew is the maximum of the cell skewness and the above quantities

computed for each face.

Note

When the cell is located on the boundary, the vector

across the boundary face is ignored

during the quality computation.

When the cell is separated from the adjacent cell by an internal wall, the vector

across

the internal boundary face is ignored during the quality computation.

When the adjacent cells share a parent-child relation, the vector

is the vector from the

cell centroid to the centroid of the child face while the vector

is the vector from the cell

centroid to the centroid of the adjacent child cell sharing the child face.

The ortho skew quality for faces is similarly computed using the edge normal vector,

, and the

vector from the face centroid to the centroid of each edge,

. Figure . : Vectors Used to Compute

Ortho Skew Quality for a Face (p. ) illustrates the vectors used to determine the ortho skew

quality for a face.

Figure . : Vectors Used to Compute Ortho Skew Quality for a Face

The ortho skew for a face is the maximum of the computed values for ( - the cosine of the angle

between the edge normal vector and the vector from the centroid of the face to the centroid of

the edge), for each edge :

(.)

Fluent Aspect Ratio

(.)

The Fluent aspect ratio is a measure of the stretching of a cell. It is computed as the ratio of the maximum

value to the minimum value of any of the following distances: the normal distances between the cell

centroid and face centroids, and the distances between the cell centroid and nodes. For a unit cube (see

Figure . : Calculating the Fluent Aspect Ratio for a Unit Cube (p. )), the maximum distance is .,

and the minimum distance is ., so the aspect ratio is ..This type of definition can be applied on

any type of mesh, including polyhedral.

Figure . : Calculating the Fluent Aspect Ratio for a Unit Cube

Inverse Orthogonal Quality

The inverse orthogonal quality for a cell is computed using the face normal vector,

for each face; the

vector from the cell centroid to the centroid of each of the adjacent cells,

; and the vector from the cell

centroid to the centroid of each face,

(see Figure . :Vectors Used to Compute Ortho Skew/Inverse

Orthogonal Quality for a Cell (p. )). For each face, the cosines of the angle between

and

, and

between

and

are calculated.The smallest calculated cosine value is the orthogonality of the cell.

Then, inverse orthogonality is found by subtracting this cosine value from .

Finally, Inverse Orthogonal Quality depends on cell type:

For tetrahedral, prism, and pyramid cells, Inverse Orthogonal Quality is the maximum of the cell

skewness and the inverse orthogonality.

For hexahedral and polyhedral cells, Inverse Orthogonal Quality is the same as the inverse ortho-

gonality.

gonality.

The worst cells will have an Inverse Orthogonal Quality closer to  and the best cells will have an

Inverse Orthogonal Quality closer to .

Note

Inverse Orthogonal Quality =  - Orthogonal Quality

Orthogonal Quality can be reported using the Quality option in the ribbon or the

Report Quality button in the General task page in solution mode (refer to Mesh

Quality (p. ) for details).

The mouse probe print function displays information about individual components of the mesh. The

type of information is determined by the selected mouse probe filter.

The print-info command reports information about an individual mesh entity (that is, a node, face,

or cell). In some circumstances, the information includes prefixes or punctuation to identify the inform-

ation type. An entity is identified by its prefix with an index value. Valid prefixes are: bn (boundary

node), n (node), bf (boundary face), f (face), and c (cell). Hence, the first boundary node would be

bn1.

The output for some of the entity types is as explained in this section.

cell

The following information is listed for a cell:

zone ID

the nodes forming the cell

the faces forming the cell

the size

the coordinates of the circumcenter (relevant for tetrahedral cells only)

square of the circumcenter radius (relevant for tetrahedral cells only)

the quality of the cell

c26 = ( (n262 n34 bn204 bn205) (f4743 f5372 f1822 f3426)

. (. . .)

. .)

The default measure of quality is skewness, but you can use the Quality Measure dialog box to specify

aspect ratio or change in size instead.

face

. (. . .)

. .)

face

The following information is listed for a face:

associated zone ID

the nodes forming the face

the neighboring cells

f32 = ( (n95 bn197 n90) (c4599 c1279))

Due to the manner in which the algorithm maintains memory, not all indices will have values—that is,

an empty slot can be caused by a delete operation. Empty slots are reused in subsequent operations,

so the actual entity at a particular index may change as the mesh is generated.

boundary face

The following information is listed for a boundary face:

the periodic shadow (null if not periodic)

the quality of the face

bf17 = ( (bn1308 bn1314 bn1272) (() c1533) () .)

node

The following information is listed for a node:

Cartesian coordinates of the node

the node radius

n30 = ( (. . .) .)

For interior nodes, the node radius is the distance-weighted average to the surrounding nodes.

boundary node

The following information is listed for the boundary node:

node radius

faces using the node.

bn1 = ( (  ) . (bf2099 bf1093 bf193))

For boundary nodes, the node radius is the average distance to neighboring boundary nodes.

Reporting Mesh Information

Appendix A. Importing Boundary and Volume Meshes

The volume-mesh generation scheme requires sets of triangular and/or quadrilateral elements defining

the boundaries of the computational domain. In addition to the basic capability provided in GAMBIT,

Fluent can use other popular CAD/CAE software packages.

A.. GAMBIT Meshes

A..TetraMesher Volume Mesh

A.. Meshes from Third-Party CAD Packages

GAMBIT can create both surface and volume meshes. See the GAMBIT Modeling Guide for details.

ICEM CFD Engineering writes a RAMPANT file from TetraMesher. TetraMesher generates tetrahedral

volume grids using a recursive subdivision octree scheme.

To read a RAMPANT file, use the File → Read → Mesh menu item or the file/read-mesh text

command.

You can import grid files from third-party CAD packages by using the items in the File → Import menu.

Alternatively, the fe2ram filter enables you to convert files created by several finite-element packages

to the grid file format used by Fluent. You can convert surface or volume meshes from ANSYS, I-deas,

NASTRAN, PATRAN, VRML files from VRML version ., or other packages. ARIES files can be converted

only if they are first saved as ANSYS Prep7 files, as described in ARIES Files (p. ).

If you choose to convert the file manually before reading it, enter the following command:

utility fe2ram [dimension] read-format [merge] [zoning] [write-format] input-file output-file

The items in square brackets are optional.

dimension indicates the dimension of the dataset.

– For a 3D grid, do not specify dimension as 3D is the default.

– For a 2D grid, replace dimension by -d2.

– For a surface mesh, replace dimension by -surface.

read-format indicates the format of the file you want to convert. Replace read-format as follows:

– For an ANSYS file, use -tANSYS.

– For an I-deas file, use -tIDEAS.

– For a NASTRAN file, use -tNASTRAN.

– For a PATRAN file, use -tPATRAN.

For a list of conversion capabilities from other CAD packages, type utility fe2ram -cl -help.

merge indicates the grid tolerance.The default is - (.0e-).To set another tolerance value, replace

merge by -mTOLERANCE, where TOLERANCE is an appropriate real number value.To reset the tolerance

to the default value, replace merge by -m.

zoning indicates how zones were identified in the CAD package. Replace zoning as follows:

– For a grid zoned by group, do not specify zoning as zoning by groups is the default.

– For a grid that was zoned by property IDs, use -zID.

– To ignore all zone groupings, use -zNONE.

write-format indicates the output format for the file you want to convert. Replace write-format as

follows:

– To write the grid for use in Fluent, do not specify write-format as this is the default.

– To write the grid in FIDAP format, use -oFIDAP7.

input-file and output-file are the names of the original file and the file to which you want to write

the converted grid information, respectively.

For example, to convert the 2D I-deas volume mesh file sample.unv to an output file called

sample.msh, enter:

utility fe2ram -d2 -tIDEAS sample.unv sample.msh

After the output file has been written, you can read it using File → Import in the meshing mode of

Fluent. For volume meshes, the resulting output file can also be read into the solution mode of Fluent.

Important

All boundary types are considered to be wall zones. You can set the appropriate boundary

types in meshing mode or in solution mode.

Note

The fe2ram utility supports VRML files from VRML version ..

A... I-deas Universal Files

For I-deas surface meshes, the filter reads triangular and quadrilateral elements that define the

boundaries of the domain and have been grouped within I-deas to create zones. For volume meshes,

the filter reads a 2D or 3D mesh that has its boundary nodes or 2D boundary elements appropriately

Importing Boundary and Volume Meshes

grouped to create boundary zones. Do not include nodes and boundary elements in the same group.

All boundary zones will be considered wall zones; you can set the appropriate boundary types in the

meshing mode or in the solution mode. See Meshes from Third-Party CAD Packages (p. ) for further

details.

A.... Recognized I-deas Datasets

The following Universal file datasets are recognized by the grid filter:

Node Coordinates

dataset number , ,

Elements

dataset number  or

Permanent Groups

dataset number , , , , ,

Because Fluent uses linear elements, you should use linear elements to generate the grid inside the

mesh areas. If parabolic elements exist in the dataset, the filter ignores the mid side nodes. This as-

sumption is valid if the edges of the element are near linear. However, if this is not the case, an incor-

rect topology may result from this assumption. For example, in regions of high curvature the parabolic

element may look much different than the linear element.

For volume meshes, note that mesh area/mesh volume datasets are not recognized. This implies that

writing multiple mesh areas/mesh volumes to a single Universal file may confuse fe2ram or Fluent.

A.... Grouping Elements to Create Zones for a Surface Mesh

The Group command in I-deas is used to create the boundary zones needed by Fluent. All faces

grouped together are listed together in the output as a single zone. In Fluent, boundary conditions

are set on a per-zone basis.

One technique is to generate groups automatically based on mesh areas—that is, every mesh area

will be a different zone. Although this method may generate a large number of zones, the zones can

be merged in the meshing mode or in the solution mode of Fluent. Another technique is to create

a group of elements related to a given mesh area manually. This enables you to select multiple mesh

areas for one group.

A.... Grouping Nodes to Create Zones for a Volume Mesh

The Group command is used in I-deas to create the boundary zones needed by Fluent. All nodes

grouped together are listed together in the output as a single zone. It is important not to group

nodes of internal faces with nodes of boundary faces.

One technique is to generate groups automatically based on curves or mesh areas—that is, every

curve or mesh area will be a different zone in Fluent. Another technique is to create the groups

manually, generating groups consisting of all nodes related to a given mesh area (3D).

Meshes from Third-Party CAD Packages

A.... Periodic Boundaries

In general, it is difficult to generate a valid grid with periodic boundaries in I-deas. However, a special

feature exists in the meshing mode in Fluent that enables you to generate a grid in a domain with

periodic boundaries. See Creating Periodic Boundaries (p. ) for further details.

A.... Deleting Duplicate Nodes

I-deas often generates duplicate nodes in the process of creating triangular elements. These must be

removed by using either the remove coincident node command in I-deas or the Merge button in the

Merge Boundary Nodes dialog box (or the /boundary/merge-duplicates text command).

This node merging process is usually faster in the meshing mode in Fluent but more visual in I-deas.

A... PATRAN Neutral Files

For PATRAN surface meshes, the filter reads triangular and quadrilateral linear elements that define

the boundaries of the domain and have been grouped by named component or identified by property

IDs within PATRAN to create zones. For volume meshes, the filter reads a 2D or 3D mesh that has its

boundary nodes grouped by named component to create boundary zones. All boundary zones will

be considered wall zones; you can set the appropriate boundary types in the meshing mode or in the

solution mode of Fluent. See Meshes from Third-Party CAD Packages (p. ) for details.

A.... Recognized PATRAN Datasets

The following Neutral file datasets are recognized by the grid filter:

Node Data

Packet Type

Element Data

Distributed Load Data

Node Temperature Data

Name Components

File Header

A.... Grouping Elements to Create Zones

In PATRAN, named components are applied to the nodes to create groups of faces called zones. In

Fluent, boundary conditions are applied to each zone. For example, all nodes on a curve or patch

can be put in a Name Component.

For 2D volume meshes, an additional constraint is placed on the elements: existence in the Z= plane.

In general, it is difficult to generate a valid grid with periodic boundaries in PATRAN. However, a

special feature exists in the meshing mode in Fluent that enables you to generate a grid in a domain

with periodic boundaries. See Creating Periodic Boundaries (p. ) for further details.

A... ANSYS Files

For ANSYS surface meshes, the filter reads triangular and quadrilateral linear elements that define the

boundaries of the domain and have been grouped within ANSYS using node and element selection.

For volume meshes, the filter reads a 2D or 3D mesh that has its boundary nodes grouped within

ANSYS using node and element selection. All boundary zones will be considered wall zones; you can

set the appropriate boundary types in the meshing mode or in the solution mode in Fluent. See Meshes

from Third-Party CAD Packages (p. ) for details.

A.... Recognized Datasets

The following datasets are recognized by the grid filter:

NBLOCK

node block data

EBLOCK

element block data

CMBLOCK

element/node grouping

The elements must be STIF63 linear shell elements. In addition, if element data without an explicit

NBLOCK

EBLOCK

CMBLOCK

element ID is used, the filter assumes sequential numbering of the elements when creating the zones.

In general, it is difficult to generate a valid grid with periodic boundaries in ANSYS. However, a special

A... ARIES Files

ARIES provides a filter or you may write a Prep7 file from ARIES and use the fe2ram filter with argu-

ments for an ANSYS file. For more information on importing ANSYS files, see ANSYS Files (p. ).

In general, to write a Prep7 file within ARIES the following criteria must be met:

Name the part in the Geom module.

Create a material or read one from the mat_lib in the Material module.To create a material, you must

supply density, Poisson’s ratio, and elastic modulus.

Generate face pressures for the surface in the Environment module. Later, when you write the Prep7 file,

these will be transferred to the individual elements.

Generate at least one restraint in the Environment module.

Set the element type to be STIF63 (triangular shell elements) and specify some finite thickness.

Write the Prep7 file, making sure you let it automatically assign the pressure to the elements.

You can filter the Prep7 file by using the ARIES or Fluent filter, whichever you find most convenient.

A... NASTRAN Files

For NASTRAN surface meshes, the filter reads triangular and quadrilateral linear elements that define

the boundaries of the solution domain. For volume meshes, the filter reads a 2D or 3D mesh. All

boundary zones are considered wall zones; you can set the appropriate boundary types in the meshing

mode or in the solution mode in Fluent. For details, see Meshes from Third-Party CAD Packages (p. ).

A.... Recognized NASTRAN Bulk Data Entries

The following NASTRAN bulk entries are recognized by the grid filter:

GRID

single-precision node coordinates

GRID*

double-precision node coordinates

CBAR

line elements

CTETRA, CTRIA3

tetrahedral and triangular elements

CHEXA, CQUAD4, CPENTA

hexahedral, quadrilateral, and wedge elements

Because Fluent uses linear elements, you should use linear elements in the mesh-generation process.

If parabolic elements exist in the dataset, the filter ignores the mid-side nodes. This assumption is

valid if the edges of the element are near linear. However, if this is not the case, an incorrect topology

may result from this assumption. For example, in regions of high curvature the parabolic element

may look much different than the linear element.

In general, it is difficult to generate a valid grid with periodic boundaries in NASTRAN. However, a

with periodic boundaries. For details, see Creating Periodic Boundaries (p. ).

NASTRAN often generates duplicate nodes in the process of creating triangular elements. You must

remove them by clicking Merge in the Merge Boundary Nodes dialog box (or by using the

/boundary/merge-duplicates text command).

Appendix B. Mesh File Format

The content and format of Fluent mesh files is described in the following sections:

B.. Guidelines

B.. Formatting Conventions in Binary Files and Formatted Files

B.. Grid Sections

B.. Non-Grid Sections

B.. Example Files

Note

A mesh file is a subset of a case file; it contains only those sections of the case file that pertain

to the mesh. The currently defined sections relevant for the mesh file are explained in the

following sections. For information about sections in the case file, refer to Grid Sections (p. )

and Other (Non-Grid) Case Sections (p. ) in the Fluent User's Guide (p. ).

The mesh files are broken into several sections according to the following guidelines:

Each section is enclosed in parentheses and begins with a decimal integer indicating its type.This integer

is different for formatted and binary files (see Formatting Conventions in Binary Files and Formatted

All groups of items are enclosed in parentheses.This makes skipping to ends of (sub)sections and parsing

them very easy. It also allows for easy and compatible addition of new items in future releases.

Header information for lists of items is enclosed in separate sets of parentheses, preceding the items, which

are in their own parentheses.

For formatted files, examples of file sections are given in Grid Sections (p. ) and Non-Grid Sec-

tions (p. ). For binary files, the header indices described in subsequent sections (for example,  for

the node section) are preceded by  for single-precision binary data, or by  for double-precision

binary data (that is,  or  instead of ). The end of the binary data is indicated by End of

Binary Section  or End of Binary Section  before the closing parameters of

the section.

An example with the binary data represented by periods is as follows:

( (  2aad  )(

.

.

.

)

End of Binary Section )

Grid sections are stored in the case file. A mesh file is a subset of a case file, containing only those sections

pertaining to the mesh. The currently defined grid sections are explained in the following sections.

B... Comment

B... Header

B... Dimensions

B... Nodes

B... Periodic Shadow Faces

B... Cells

B... Faces

B... Edges

B... Face Tree

B... Cell Tree

B... Interface Face Parents

The section ID numbers are indicated in both symbolic and numeric forms. The symbolic representations

are available as symbols in a Scheme source file (xfile.scm), which is available from ANSYS, Inc., or

as macros in a C header file (xfile.h), which is located in your installation area.

Index:

xf-comment

Scheme symbol:

XF_COMMENT

C macro:

optional

Status:

Comment sections can appear anywhere in the file (except within other sections) as:

( "comment text")

You should precede each long section or group of related sections, by a comment section explaining

what is to follow.

For example,

( "Variables:")

( (

(max-skew-limit .)

(max-cell-skew .)

(skewness-method )

))

Index:

xf-header

XF_HEADER

C macro:

optional

Status:

Mesh File Format

( (

))

Index:

xf-header

XF_HEADER

C macro:

optional

Status:

Header sections can appear anywhere in the file (except within other sections). The following is an

example:

( "ANSYS(R) TGrid(TM) 3D, serial ..")

The purpose of this section is to identify the program that wrote the file. Although this section can

appear anywhere, it is typically one of the first sections in the file. Additional header sections indicate

other programs that may have been used in generating the file. This provides a history mechanism

showing where the file came from and how it was processed.

Index:

xf-dimension

XF_DIMENSION

C macro:

optional

Status:

The dimensions of the grid appear as:

( ND)

where ND is  or . This section is supported as a check that the grid has the appropriate dimensions.

B... Nodes

Index:

xf-node

XF_NODE

C macro:

required

Status:

The nodes section appears as:

( (zone-id first-index last-index type ND)(

x1 y1 z1

x2 y2 z2

.

.

.

))

If zone-id is zero, this provides the total number of nodes in the mesh. In this case, first-index will

be one, last-index will be the total number of nodes in hexadecimal, type is zero, ND is omitted, and

there are no coordinates following (the parentheses for the coordinates are omitted as well).

( (  2d5 ))

If zone-id is greater than zero, it indicates the zone to which the nodes belong. In this case, first-

index and last-index are the indices of the nodes in the zone in hexadecimal.The values of last-

index in each zone must be less than or equal to the value in the declaration section. type indicates the

type of nodes in the zone.The following values are used to indicate the node type:

Grid Sections

– Zero for “virtual” nodes.

– One for no (any) type.

– Two for boundary nodes.

Nodes of type zero are ignored but types one and two are read and written.

ND is an optional argument that indicates the dimensionality of the node data, where ND is  or .

If the number of dimensions in the grid is two, as specified in the Dimensions (p. ) or in the node

header, then only x and y coordinates are present on each line.

The following is an example of a two-dimensional grid:

( (  2d5  )(

.500000e- .500000e-

.625000e- .250000e-

.

.

.

.750000e- .000000e+

.000000e- .500000e-

.875000e- .250000e-

))

As the grid connectivity is composed of integers representing pointers (see Cells (p. ) and

Faces (p. )), using hexadecimal conserves space in the file and provides for faster file input and

output. The header indices are also in hexadecimal so that they match the indices in the bodies of the

grid connectivity sections. The zone-id and type are also in hexadecimal for consistency.

Index:

xf-periodic-face

XF_PERIODIC_FACE

C macro:

required only for grids with periodic

boundaries

Status:

This section indicates the pairings of periodic faces on periodic boundaries. Grids without periodic

boundaries do not have sections of this type.

The format of the section is as follows:

( (first-index last-index periodic-zone shadow-zone)(

f00 f01

f10 f11

f20 f21

.

.

.

))

where:

first-index is the index of the first periodic face pair in the list.

last-index is the index of the last periodic face pair in the list.

f00 f01

f10 f11

f20 f21

.

.

.

))

where:

periodic-zone is the zone ID of the periodic face zone.

shadow-zone is the zone ID of the corresponding shadow face zone.

These are in hexadecimal format.

The indices in the section body (f*) refer to the faces on each of the periodic boundaries (in hexa-

decimal), the indices being offsets into the list of faces for the grid.

Note

The first-index and last-index do not refer to face indices; they refer to indices in

the list of periodic pairs.

An example of such a section is as follows:

( ( 2b a c) (

1f

ad 1c2

.

.

.

))

B... Cells

Index:

xf-cell

XF_CELL

C macro:

required

Status:

The declaration section for cells is similar to that for nodes.

( (zone-id first-index last-index type element-type))

When zone-id is zero, it indicates that it is a declaration of the total number of cells. If last-index

is zero, then there are no cells in the grid. This is useful when the file contains only a surface mesh as

it serves to alert Fluent that it cannot be used in the solver.

In a declaration section, the type has a value of zero, while the element-type is not present.

( (  3e3 ))

states that there are 3e3 (hexadecimal) =  cells in the grid. This declaration section is required and

must precede the regular cell sections.

The element-type in a regular cell section header indicates the type of cells in the section, as follows:

faces/cell

nodes/cell

description

element-type

mixed

triangular

quadrilateral

hexahedral

pyramid

wedge

NF

mixed

pyramid

wedge

NF

NN

polyhedral

where NN and NF will vary, depending on the specific polyhedral cell.

Regular cell sections have no body, but they have a header of the same format where first-index

and last-index indicate the range for the particular zone, type indicates whether the cell zone is

fluid (type = ) or solid (type = ).

A type of zero indicates a dead zone and will be skipped when the file is read in solution mode in

Fluent. If a zone is of mixed type (element-type=), it will have a body that lists the element-

type of each cell.

In the following example, there are 3d (hexadecimal) =  cells in cell zone , of which the first  are

triangles, the next  are quadrilaterals, and so on.

( (  3d  )(

.

.

.

))

Note

The cell section is not required in meshing mode when the file contains only a surface mesh.

B... Faces

Index:

xf-face

XF_FACE

C macro:

required

Status:

The face section has a header with the same format as that for cells, but with a section index of .

The format is as follows:

( (zone-id first-index last-index bc-type face-type))

where:

zone-id = zone ID of the face section

first-index = index of the first face in the list

last-index = index of the last face in the list

bc-type = ID of the boundary condition represented by the face section

face-type = ID of the type(s) of face(s) in the section

A zone-id of zero indicates a declaration section, which provides a count of the total number of

faces in the mesh. Such a section omits the bc-type and is not followed by a body with further in-

formation.

A non-zero zone-id indicates a regular face section and will be followed by a body containing in-

formation about the grid connectivity. Each line describes one face and appears as follows:

n0 n1 n2 c0 c1

where n* are the defining nodes (vertices) of the face, and c* are the adjacent cells.

This is an example of the format for a 3D grid with a triangular face format. The actual number of

nodes depends on the face-type. The order of the cell indices is important and is determined by

the right-hand rule: if you curl the fingers of your right hand in the order of the nodes, your thumb

will point toward c0.

If the face zone is of mixed type (face-type= ) or of polygonal type (face-type= ), each line of the

section body will begin with a reference to the number of nodes that make up that particular face,

and has the following format:

x n0 n1 ... nf c0 c1

where x = number of nodes (vertices) of the face and nf is the final node of the face.

All cells, faces, and nodes have positive indices. If a face has a cell only on one side, then either c0 or

c1 is zero. For files containing only a boundary mesh, both these values are zero.

bc-type indicates the ID of the boundary condition represented by the face section. The current

valid boundary condition types are defined in the following table:

bc-type

interior

wall

pressure-inlet, inlet-vent, intake-fan

pressure-outlet, exhaust-fan, outlet-vent

symmetry

periodic-shadow

periodic

fan, porous-jump, radiator

interface

parent (hanging node)

outflow

axis

symmetry

periodic

interface

outflow

axis

The faces resulting from the intersection of the non-conformal grids are placed in a separate face zone.

A factor of  is added to the bc-type of these sections; for example,  is a wall zone.

face-type indicates the type of faces in the zone as defined in the following table:

nodes/face

face-type

mixed

linear

NN

polygonal

where NN will vary, depending on the specific polygonal face.

B... Edges

Index:

xf-edge

XF_EDGE

C macro:

optional

Status:

The edge section has a header of the following format:

where:

zone-id is the zone ID for the edge section

first-index and last-index are the index of the first and last edge in the list, respectively

type indicates the edge type

The element-type is ignored completely.

A zone-id of zero indicates a declaration section with no body, which provides a count of the total

number of edges in the mesh. A non-zero zone-id indicates a regular edge section, and will be fol-

lowed by a body containing information about the grid connectivity. Each line describes one edge

and appears as follows:

v0 v1

where v0, v1 are the vertices defining the edge.

type denotes the edge type as defined in the following table:

type

boundary edge

type

interior edge

Note

In case files written for Fluent, the Edges section will be omitted.

Index:

xf-face-tree

XF_FACE_TREE

C macro:

only for grids with hanging-node

adaption

Status:

Index:

C macro:

adaption

Status:

This section indicates the face hierarchy of the grid containing hanging nodes. The format of the section

is as follows:

( (face-id0 face-id1 parent-zone-id child-zone-id)

(

number-of-kids kid-id- kid-id- ... kid-id-n

.

.

.

))

where

face-id0 is the index of the first parent face in the section.

face-id1 is the index of the last parent face in the section.

parent-zone-id is the ID of the zone containing the parent faces

child-zone-id is the ID of the zone containing the children faces.

number-of-kids is the number of children of the parent face.

kid-id-n are the face IDs of the children.

These are in hexadecimal format. You can read files that contain this section in the meshing mode in

Fluent.

Index:

xf-cell-tree

XF_CELL_TREE

C macro:

adaption

Status:

This section indicates the cell hierarchy of the grid containing hanging nodes.

( (cell-id0 cell-id1 parent-zone-id child-zone-id)

(

.

.

.

))

where:

cell-id0 is the index of the first parent cell in the section.

cell-id1 is the index of the last parent cell in the section.

parent-zone-id is the ID of the zone containing the parent cells.

child-zone-id is the ID of the zone containing the children cells.

number-of-kids is the number of children of the parent cell.

kid-id-n are the cell IDs of the children.

These are in hexadecimal format. You cannot read files that contain this section in the meshing mode

in Fluent.

Index:

xf-face-parents

in Fluent.

Index:

XF_FACE_PARENTS

C macro:

only for grids with non-conformal

interfaces

Status:

This section indicates the relationship between the intersection faces and original faces. The intersection

faces (children) are produced from intersecting two non-conformal surfaces (parents) and are some

fraction of the original face. Each child will refer to at least one parent.

( (face-id0 face-id1)

(

parent-id- parent-id-

.

.

.

))

where:

face-id0 is the index of the first child face in the section.

face-id1 is the index of the last child face in the section.

parent-id-* is the index of the parent faces.

If you set up and save a non-conformal mesh in the solution mode and then read it into the meshing

mode of Fluent, this section will be skipped. Hence, all the information necessary to preserve the non-

conformal interface will not be maintained. When you switch to the solution mode or read the mesh

back into the solution mode, you will need to recreate the interface.

The non-grid sections contain the boundary conditions, material properties, and solver control settings.

B... Zone

B... Zone

or

Index:

xf-rp-tv

XF_RP_TV

C macro:

required

Status:

Typically, there is one zone section for each zone referenced by the grid. Although some grid zones

may not have corresponding sections, there cannot be more than one zone section for each zone.

The zone section has the following form:

( (zone-id zone-type zone-name domain-id)(

(condition1 . value1)

(condition2 . value2)

(condition3 . value3)

.

.

.

))

Grid generators and preprocessors need only provide the section header and leave the list of conditions

empty, as in:

( (zone-id zone-type zone-name domain-id)())

The empty parentheses at the end are required. The solver adds conditions as appropriate, depending

on the zone type.

When only zone-id, zone-type, zone-name, and domain-id are specified, the index  may

be used for a zone section. However, the index  must be used if boundary conditions are present,

because any and all remaining information in a section of index  after zone-id, zone-type,

zone-name, and domain-id will be ignored.

In meshing mode, the zone name and type can be extracted from the boundary condition section

(refer to the Fluent User’s Guide for details) or , but only section  can be written.

The zone-id is in decimal format. This is in contrast to the use of hexadecimal in the grid sections.

The zone-type is one of the following:

degassing

exhaust-fan

fan

fluid

geometry

inlet-vent

Non-Grid Sections

intake-fan

interface

interior

internal

outflow

outlet-vent

parent-face

porous-jump

radiator

solid

symmetry

wall

wrapper

The interior, fan, porous-jump, and radiator types can be assigned only to zones of faces

inside the domain. The interior type is used for the faces within a cell zone; the others are for in-

terior faces that form infinitely thin surfaces within the domain. Fluent allows the wall type to be

assigned to face zones both on the inside and on the boundaries of the domain.

Some zone types are valid only for certain types of grid components (for example, cell zones can be

assigned only either fluid or solid type). All other types listed can be used for only boundary (face)

zones.

The zone-name is a label for the zone. It must be a valid Scheme symbol and is written without

quotes. The rules for a valid zone-name are as follows:

The first character must be a lowercase letter or a special-initial.

Each subsequent character must be a lowercase letter, a special-initial, a digit, or a special-subsequent.

A special-initial character is one of the following:

! $ % & * / : < = > ? ~ _ ^

and a special subsequent is one of the following:

. + -

Some examples of zone sections produced in the meshing mode are as follows:

( ( fluid fuel )())

( ( pressure-inlet pressure-inlet- )())

( ( wall wing-skin )())

( ( symmetry mid-plane )())

The examples show 2D quadrilateral meshes for easier illustration. The same concepts are applied to 3D

meshes.

Example

Figure : Quadrilateral Mesh (p. ) illustrates a simple quadrilateral mesh with no periodic boundaries

or hanging nodes.

Figure : Quadrilateral Mesh

The following describes this mesh:

( "Grid:")

( "Dimensions:")

( )

( (   ))

( (  a ))

( (    ))

( (    ))

( (    )(

))

( (    )(

))

( (    )(

))

( (   a )(

))

( ( a a  )(

))

( (    )

(

.00000000e+ .00000000e+

.00000000e+ .00000000e+))

Example

Example

Figure : Quadrilateral Mesh with Periodic Boundaries (p. ) illustrates a simple quadrilateral mesh with

periodic boundaries but no hanging nodes. In this example, bf9 and bf10 are faces on the periodic

zones.

Example Files

Figure : Quadrilateral Mesh with Periodic Boundaries

( )

( "Grid:")

( (   ))

( (  a ))

( (    ))

( (    ))

( (    )(

))

( (    )(

))

( (    )(

))

( (   c )(

))

( ( a a  )(

))

( (   )(

a))

( (    )(

Example

Figure : Quadrilateral Mesh with Hanging Nodes (p. ) illustrates a simple quadrilateral mesh with

hanging nodes.

Figure : Quadrilateral Mesh with Hanging Nodes

( "Grid:")

( )

( (   ))

( (   ))

( (  d  ))

( (    ))

( (    ))

( (   )(

))

( (    )(

))

( (  b  )(

a

b

))

( ( c f  )(

c

d  ))

( (   a )(

d a  ))

( (    )(

c

b   ))

( (b   1f )(

c   ))

( (a   1f )(

b c  ))

( (   1f )(

b  ))

( (   1f )(

))

( (  b )(

d c))

( (  a )(

))

( (   )(

b a))

( (   )(

))

( (  d  )

(

.50000000e+ .00000000e-

.50000000e+ .00000000e+

.00000000e+ .00000000e-

Appendix C. Shortcut Keys

Creating a mesh and modifying or repairing it involves many operations. Various tools are available for

making boundary repairs, enabling you to perform primitive operations on the boundary mesh, such

as creating and deleting nodes/faces; moving nodes; swapping edges; merging/smoothing nodes; col-

lapsing nodes, edges, and faces; and so on.

You can perform these operations using the appropriate dialog boxes. However, if you are handling a

large and complicated mesh, you may find it difficult to perform these operations repetitively using the

dialog boxes. To make your task easy, keyboard shortcuts are available.

C.. Shortcut Key Actions

Important

To make use of the keyboard shortcuts, display the geometry in the graphics window, click

in the graphics window, then press the key combination. Many of the keyboard shortcuts

are available as an onscreen tool button along the left side and bottom of the graphics

window.

To repeat the same shortcut multiple times, after pressing the key combination, press Ctrl

while using the right mouse button for multiple selections. This repeat shortcut is available

only for some operations. The hot key help indicates the (previous) operation that will be

performed in case of multiple selections.

Onscreen Tool

Keys

Action

Feature

Ctrl+H

Print the available hot keys in the message and

Hot key list

Ctrl+B

Selection

filters

CAD Entities

Note

Some

Keys

Ctrl+Z

CAD zone filter

Ctrl+X

Ctrl+B

Selection

filters

Note

Some

Keys

Ctrl+Z

Ctrl+X

and

Onscreen

F6

Highlight parent CAD object

Display

options

Tools

may

F7

Highlight child CAD object

Ctrl+Shift+C

Color by labels

have

different

Ctrl+Shift+D

Color by threads

behavior

Ctrl+C

Isolate similar curvature

Isolate tools

for

CAD

Keys

Action

Feature

Assemblies

and

Ctrl+L

Isolate smaller area

Ctrl+S

Isolate similar area

Geometry/Mesh

Objects.

Ctrl+G

Delete inactive/suppressed CAD

objects

Tree

options

Ctrl+Y

Clear CAD tree selections

Ctrl+Shift+P

Show CAD object path

Ctrl+P

Add to object

Object

management

Ctrl+Q

Replace object

Ctrl+Shift+B

Create objects

Ctrl+Shift+L

Manage labels

Label

Ctrl+I

CAD zone associated labels

Ctrl+Shift+F

Extract edge zones

Modify

Ctrl+Shift+N

Rename CAD objects

Ctrl+Shift+R

Update CAD objects

Ctrl+Shift+S

Suppress CAD objects

Ctrl+J

Restore deleted nodes

Up arrow

Increase

Display

bounds

Down ar-

row

Decrease

Ctrl+L

Prints the coordinates of the centroid of the

selected face to the console.

Faces

Rezones the selected faces/cells to the target zone. Ctrl+O

Apply after setting a target zone and selecting

source face(s) or cell(s).

Ctrl+Shift+J

Mark faces based on selections and specified

parameters. Marking faces allows for selective

separation or remeshing.

If help text display is active, a description of

the marking options is displayed.

Shortcut Keys

Keys

Action

Feature

Ctrl+S

Mark selected faces.

Marking

options

Ctrl+D

Mark faces by flood filling.

Ctrl+R

Keys

Action

Feature

Ctrl+S

Marking

options

Ctrl+D

Ctrl+R

Mark faces in rings around selection.

Ctrl+Q

Mark faces by quality.

Ctrl+G

Mark faces by angle.

Ctrl+L

Mark island faces.

Ctrl+U

Unmark all/selected marked faces

Ctrl+I

Opens the Mark Settings dialog

box, where you can set the

parameters for marking faces.

Open the Local Remesh or Zone Remesh dialog

box to set options and remesh faces (or zones)

based on your selection in the graphics window.

Face selection will remesh the face and specified

radial layers based on settings in the Local

Remesh dialog box.

Face zone selection will remesh the zone based

on settings in the Zone Remesh dialog box.

No selection will remesh marked faces.

Separates the face or edge zones based on the

selected entity.

If a multi-region face zone is selected, then the

face zones are separated by region.

If a single region face zone is selected, then the

face zones are separated by angle.

If a face (or edge) is selected, then the face zone

(edge zone) is separated by seed.

If edge zone with face seed selection, then the

face zone is separated by edge loop.

If no selection, then the face zones are separated

by mark.

Opens the Create Edge Zones dialog box to extract

the edges of the surface(s) containing the selected

face(s). See Extract Edge Zones (p. ).

Show/hide edges on selected zones and objects

independent of the mode of selection.If no

Edges

object/zone is selected, then the edges on the

entire geometry are shown/hidden.

Prints the coordinates of the center of the selected Ctrl+L

edge to the console.

Edges

This also works for faces and nodes.

Shortcut Key Actions

Keys

Action

Feature

Right ar-

row

Display in decreasing order of skewness in the

mesh/active group or the marked faces.

Skewed faces

Left arrow

Clear

F3

Toggle between the mouse-dolly and the option

currently selected for the right-mouse button.

Mouse But-

tons dialog

box

or

or

F4

Toggle the selection of the mouse probe function

between polygon and the option currently

selected in the Mouse Probe dialog box.

Note

When using box select or polygon

select, by default, all entities

Mouse Probe

(nodes, faces, zones, objects) will

be selected.

To select only visible entities

instead, enable Select Visible En-

tities in the Mouse Probe Func-

tions group in the ribbon.

If the mesh is not connected, all

entities (nodes, faces, zones, objects)

will be selected irrespective of

whether they are visible or not.

This visual selection behavior works

only on local displays and may

generate warning messages when

attempting selection on a remote

system.

Ctrl+B

Select object as the selection filter.

Ctrl+C

Select cell as the selection filter.

This works only in the Linux version.

Ctrl+E

Select edge as the selection filter.

Ctrl+F

Select face as the selection filter.

Ctrl+N

Select node as the selection filter.

Ctrl+X

Select position as the selection filter.

Keys

Action

Feature

Ctrl+Y

Select size based on the computed size field as

the selection filter.

Ctrl+Z

Select zone as the selection filter.

F5

Create the selected entity.

Entities

F6

Keys

Action

Feature

Ctrl+Y

Ctrl+Z

F5

Entities

F6

Smooth the selected entity.

F7

Perform the split operation on the selected entity

(only face and edge).

F8

Perform the swap operation on the selected entity

F9

Merge the selected pair.

Ctrl+J

Alternatively,

Ctrl+^

Perform the collapse operation on the selected

nodes, edges, or faces.

Ctrl+W

Delete the selected entities

(nodes/faces/zones/objects) without confirming.

Ctrl+Shift+Z

Toggle Edge Zone selection mode. This restricts

selection to edge zones entities only.

Hide the selected objects or zones

in the display depending on the

mode of selection set.

Viewing

options

only. These

do not

Isolate selected zones/objects.

affect the

mesh.

Ctrl+Shift+U

Reverse the last show/hide

Ctrl+I

Print detailed information

about the selected entities in

the message window. For more

details, see Entity

Information (p. ).

In addition, if a selected zone

or object has been set as a

target, this hotkey, or tool

button, will toggle the

Ctrl+[

Alternatively:

Esc

Deselect the last selected entity.

Keys

Action

Feature

F2

Clear all selection and visualization

assists.

Show all hidden zones/objects;

show previously hidden

zones/objects.

Ctrl+D

Calculate and display the distance

between the two selected entities.

The value is also printed in the

console window.

Ctrl+G

Displays the neighboring face zones

of the selected entity.

Ctrl+V

Move nodes from their original location to a new

position.

Nodes

Ctrl+L

Ctrl+G

Ctrl+V

position.

Nodes

Ctrl+L

Prints the coordinates of the selected node to the

console.

F11

Show only the worst skewed face and its ID; print

the skewness value in the console.

Mesh/active

group

F12

Undo latest operation (if possible).

Mesh

operation

Ctrl+A

Adjust to fit in the graphics window.

Mesh display

Ctrl+K

Remove Boundary Gaps. Apply after setting a

target zone and selecting a source zone.

Objects

Ctrl+Shift+M

Merge all the selected objects/zones into one

object/zone depending on which mode of

selection is set.

For object selection, only objects of the same

type (geometry or mesh) can be merged. Enter

a name for the merged object in the Merge Ob-

jects dialog box.

For zone selection, only zones of the same type

or belonging to the same object can be merged.

The resulting zone inherits the name of the zone

selected first.

Open the Change Object Properties or Change

Zone Properties dialog box, depending on your

selection.

Ctrl+Shift+O

Randomly allocates colors to selected

objects/zones, or, if no object/zone is selected, to

Expands the on-screen selection

tools menu.

Selection

Tools

Graphics

window

Keys

Action

Feature

Selects the object at the mouse

pointer.

Click and drag to select objects

within a rectangular box.

Click repeatedly to define an object

selection polygon.

Ctrl+Shift+V

Selects all the visible objects/zones

in the graphics window.

Ctrl+_

Display the previous view.

Ctrl+[

Esc

Ctrl+Shift+G

Align objects.

Ctrl+_

Ctrl+[

Esc

Visualization

Tools

Expands the on-screen Viewing

tools menu

Ctrl+Shift+X

Toggle between a normal view and

an exploded view of the objects in

the geometry.

Ctrl+Shift+T

Toggle the transparency of the

selected objects/zones depending

on the mode of selection set. If no

object/zone is selected then the

entire geometry is made transparent

so that internal objects/zones are

visible.

Displays objects with similar

curvature as the current selection.

Ctrl+D

The value is also printed in

the console window.

Keys

Action

Feature

Preview size field at selected

location.

Displays objects with similar area as

the current selection.

Displays objects with smaller area

than the current selection.

Ctrl+S

Set/Unset a projection target. The target will

be a line, plane, zone, or object depending

on the selection.

Projection

The target is used for easy object modification,

for rezoning of faces/cells, for projecting

nodes or zones, or for gap removal.

the target options is displayed.

Ctrl+P

Project selected nodes/node loops/zones onto

what you have set using Ctrl+S.

Displays information about the selected target and Ctrl+I

Ctrl+P

toggles the identifying target color.

Ctrl+R

Auto patch zones by filling all holes based on

the selected entity. Select the face zone to

patch all holes associated with free faces.

Zones

Select individual faces adjacent to the hole in

the face zone to patch punched holes. See

the User's Guide (p. ) for details.

Open the Change Object Properties or

Change Zone Properties dialog box,

depending on the selection of objects or

zones in the graphics window.

If zones are graphically selected, they are remeshed Ctrl+Shift+R

using the size field, if available.

Ctrl+Shift+Y

Transfer the selected zone(s) to the target object,

if applied after setting a target object and selecting

source zone(s). If no target is set, the selected

zone(s) will form a new geometry object as

specified in the Create Geometry Object dialog

box.

edges of the selected face zone. See Extract Edge

Zones (p. ).

Ctrl+Shift+K

Enter the Construct Geometry mode to create a

bounding box, cylinder, or frustum for selected or

all zones displayed in the graphics window.

Construct

geometry

primitives

Ctrl+B

Create a bounding box for selected/all displayed

zones.

Keys

Action

Feature

Ctrl+C

Create a cylinder based on selections or bounding

all displayed zones.

Ctrl+F

Create a frustum based on selections or bounding

F5

Open the Create Object dialog box to specify

additional settings. Click Create to create the

geometry object based on the selections and

settings.

F5

settings.

Enter the Loop Selection Mode. Select a loop of

nodes/positions for probe selection or for creating

an edge loop or capping surface.

Loop of

nodes

Select position for loop creation.

Selection

options

Ctrl+O

Toggle between an open or closed

loop.

Ctrl+D

Toggle between

using the direct

or node loop

Closed loop

options

closing path

between the first

and last nodes.

Ctrl+E

or feature path

Ctrl+B

or zone

boundary path

Ctrl+P

Toggle between using the node

path or the direct path between the

last two nodes selected.

Ctrl+F

Toggle between using the feature

Ctrl+Z

Toggle between using the zone

boundary path or the direct path

between the last two nodes

selected.

Ctrl+J

Select all nodes on the loop path.

Create

options

Keys

Action

Feature

Ctrl+K

Create a capping surface based on

the nodes selected.

Ctrl+L

Create an edge loop based on the

nodes selected.

Enter List Selection options mode.

List Selection

Options

mode

Contains options for controlling selection lists

in dialog boxes based on zones or objects

selected in the graphics window. You can also

select face zone labels in the tree based on

zones selected in the graphics window.

Ctrl+Q

Add the selected zones to the

current selections in the dialog box

list.

Zone

selection

Remove the selected zones from the Ctrl+S

Ctrl+Q

list.

Zone

selection

list.

Ctrl+D

Set the selected zones as the

list.

Ctrl+J

Add the selected objects to the

list.

Object

selection

Ctrl+K

Remove the selected objects from

the current selections in the dialog

box list.

Ctrl+L

Set the selected objects as the

list.

Ctrl+F

Add the face zone labels

corresponding to zones selected to

the current selections in the tree.

Face Zone

Label

selection

Ctrl+G

Remove the face zone labels

corresponding to zones selected

from the current selections in the

tree.

Ctrl+R

Set the face zone labels

corresponding to zones selected as

F2

Exit list selection options mode.

Enter the Color Options mode.

Color Options

mode

Ctrl+G

Color the items by geometry recovery attribute.

Ctrl+O

Color the items by object.

Ctrl+Z

Color the items by zone.

Ctrl+N

Color the items based on normals.

Keys

Action

Feature

Ctrl+P

Toggle the color palette.

Ctrl+R

Randomize the colors used in the display.

F2

Exit color options mode.

Enter the Conditional Display Options mode.

Conditional

Display

Ctrl+S

Isolate zones/objects with similar surface area to

selected.

Options

mode

Ctrl+I

Isolate zones/objects with surface area less than

or equal to selected.

Ctrl+C

Isolate zones/objects of similar surface curvature.

Ctrl+N

Isolate zones/objects with neighborhood.

Ctrl+C

Ctrl+N

Show all zones/objects in the graphics window;

unhide previously hidden zones/objects.

F2

Exit conditional display options mode.

Ctrl+T

Enter the Miscellaneous Tools mode.

Miscellaneous

Tools mode

Ctrl+P

Preview sizes on selected/all zones.

Ctrl+C

Draw size contours on selected/all zones.

Ctrl+T

Trace path between selected entities.

Ctrl+J

Join selected face zones using the options in the

Join dialog box.

Ctrl+I

Intersect selected face zones using the options in

the Intersect dialog box.

Enables you to improve feature capture and/or

rezone wrap face zones.

Wrap face

zones

When wrap face zones are selected, they are

rezoned.

When wrap face zones and edge zones are

selected, feature capture on the wrap face zones

is improved and the face zones are rezoned.

When wrap face zones and edge entities are

is improved.

C... Entity Information

The information displayed for the selected entities using the hot key Ctrl+I is as follows:

Information displayed

Entity selected

Zone

Zone name

Zone ID

Location

Zone type

Object that the zone is included in

Face zone labels that the zone is

included in

Regions that the zone is included in

Size functions

Face

Face name

Zone ID

Nodes

Adjoining cell(s)

Face skewness (if applicable)

Periodic twins (if applicable)

Child faces (if applicable)

Edge

Edge name

Zone ID

Adjoining faces

Cell

Cell name

Zone ID

Nodes

Faces

Cell center

Cell skewness

Cell simplex radius

Edge

Edge name

Zone ID

Cell

Cell name

Zone ID

Nodes

Faces

Cell size

Node

Node name

Zone ID

Location

Adjoining faces (if applicable)

Adjoining cells (if applicable)

Bibliography

Important

Under U.S. and international copyright law, ANSYS, Inc. is unable to distribute copies of the

papers listed in the bibliography, other than those published internally by ANSYS, Inc. Use

your library or a document delivery service to obtain copies of copyrighted papers.

[] T. J. Baker. Three Dimensional Mesh Generation By Triangulation of Arbitrary Point Sets. Technical Report

AIAA--. American Institute of Aeronautics and Astronautics. .

[] T. J. Barth. Three-Dimensional Unstructured Grid Generation via Incremental Insertion and Local Optim-

ization In Software Systems for Surface Modeling and Grid Generation. Langley Research Center,

Hampton, Virginia, NASA Conference Publication. . April .

[] K. R. Blake. A 3D Delaunay Unstructured Grid Generator Applied to Trains, Planes, and Automobiles.

Technical Report AIAA93-. American Institute of Aeronautics and Astronautics. .

[] A. Bowyer. Computing Dirichlet Tessellations. The Computer Journal. (). –. May .

[] M. Garland. Surface Simplification Using Quadric Error Metrics. 24th Annual Conference on Computer

Graphics and Interactive Techniques. –. .

[] D. G. Holmes. The Generation of Unstructured Triangular Meshes Using Delaunay Triangulation. J.

Hauser. Numerical Grid Generation in Computational Fluid Mechanics . –. Pineridge Press

Limited. .

[] Y. Kallinderis. Hybrid Prismatic/Tetrahedral Grid Generation for Complex Geometries Technical Report

Limited. .

AIAA--. AIAA 33rd Aerospace Sciences Meeting and Exhibit Reno, Nevada. .

[] Y. Kallinderis. Prismatic Grid Generation for Three-Dimensional Complex Geometries. AIAA Journal. ().

–. October .

[] L. Kobbelt. A Shrink Wrapping Approach to Remeshing Polygonal Surfaces. Computer Graphics Forum.

(). –. .

[] C. L. Lawson. Properties of n-dimensional Triangulations. Computer-Aided Geometric Design. . –.

December .

[] R. Löhner. Generation of Three-Dimensional Unstructured Grids by the Advancing Front Method Tech-

nical Report, AIAA--. American Institute of Aeronautics and Astronautics. .

[] D. J. Mavriplis. Adaptive Mesh Generation for Viscous Flows Using Delaunay Triangulation. Journal of

Computational Physics. (). –. October .

[] J. D. Müller. A Frontal Approach for Node Generation in Delaunay Triangulations. International Journal

For Numerical Methods in Fluids. (). –. August .

[] S. Pirzadeh. Unstructured Viscous Grid Generation by the Advancing-Layers Method. AIAA Journal. ().

–. August .

[] S. Pirzadeh. Three-Dimensional Unstructured Viscous Grids by the Advancing-Layers Method. AIAA

Journal. (). –. January .

[] W. R. Quadros. Finite Element Mesh Sizing for Surfaces Using Skeleton. In Proc 13th Int Meshing

Roundtable. .

[] J. Z. Wang. An Adaptive Cartesian Grid Generation Method for ‘Dirty’ Geometry. International Journal

For Numerical Methods in Fluids. . –. .

[] D. F. Watson. Computing the n-dimensional Delaunay tessellation with application to Voronoi polytopes.

The Computer Journal. (). –. May .

[] N. P. Weatherill. A Method For Generating Irregular Computational Grids in Multiply Connected Planar

Domains. International Journal For Numerical Methods in Fluids. (). – . February .

[] M. A. Yerry. Automatic Three-Dimensional Mesh Generation by the Modified-Octree Technique. Interna-

tional Journal for Numerical Methods in Engineering. . –. .

[] J. Zhu. Background Overlay Grid Size Functions. In Proc 11th Int Meshing Roundtable. .

Part III: Solution Mode

The section describes how to use ANSYS Fluent in solution mode.

Using This Manual (p. dxlv), provides typographical and mathematical conventions.

Graphical User Interface (GUI) (p. ), describes the mechanics of using the graphical user interface and the

GUI on-line help.

Text User Interface (TUI) (p. ), describes the mechanics of using the text interface and the TUI on-line help.

(See the Text Command List for information about specific text interface commands.)

Reading and Writing Files (p. ), describes the files that ANSYS Fluent can read and write, including picture

files.

Unit Systems (p. ), describes how to use the standard and custom unit systems available in ANSYS Fluent.

Fluent Expressions Language (p. ), describes how to use theANSYS Fluent Expression Language.

Reading and Manipulating Meshes (p. ), describes the various sources of computational meshes and ex-

plains how to obtain diagnostic information about the mesh and how to modify it by scaling, translating,

and other methods.This chapter also contains information about the use of non-conformal meshes.

Cell Zone and Boundary Conditions (p. ), describes the different types of boundary conditions available

in ANSYS Fluent, when to use them, how to define them, and how to define boundary profiles and volumetric

sources and fix the value of a variable in a particular region. It also contains information about porous media

and lumped parameter models.

Physical Properties (p. ), describes the physical properties of materials and the equations that ANSYS

Fluent uses to compute the properties from the information that you input.

Modeling Basic Fluid Flow (p. ), describes the governing equations and physical models used by ANSYS

Fluent to compute fluid flow (including periodic flow, swirling and rotating flows, compressible flows, and

inviscid flows), as well as the inputs you need to provide to use these models.

Modeling Flows with Moving Reference Frames (p. ), describes the use of single moving reference frames,

multiple moving reference frames, and mixing planes in ANSYS Fluent.

Modeling Flows Using Sliding and Dynamic Meshes (p. ), describes the use of sliding and deforming

meshes in ANSYS Fluent.

Modeling Turbulence (p. ), describes the use of the turbulent flow models in ANSYS Fluent.

Modeling Heat Transfer (p. ), describes the use of the physical models in ANSYS Fluent to compute heat

transfer(including convective and conductive heat transfer, natural convection, radiative heat transfer, and

periodic heat transfer), as well as the inputs you need to provide to use these models

Modeling Heat Exchangers (p. ), describes the use of the heat exchanger models in ANSYS Fluent.

Modeling Species Transport and Finite-Rate Chemistry (p. ), describes the use of the finite-rate chemistry

models in ANSYS Fluent.This chapter also provides information about modeling species transport in non-

reacting flows.

Modeling Non-Premixed Combustion (p. ), describes the use of the non-premixed combustion model in

ANSYS Fluent.This chapter includes details about using prePDF.

Modeling Premixed Combustion (p. ), describes the use of the premixed combustion model in ANSYS

Fluent.

Modeling Partially Premixed Combustion (p. ), describes the use of the partially premixed combustion

model in ANSYS Fluent.

Modeling a Composition PDF Transport Problem (p. ), describes the use of the composition PDF transport

Using Chemistry Acceleration (p. ), describes the use of methods to accelerate computations for detailed

chemical mechanisms involving laminar and turbulent flames.

Modeling Engine Ignition (p. ), describes the use of the engine ignition models in ANSYS Fluent.

Modeling Pollutant Formation (p. ), describes the use of the models for the formation of NOx, SOx, and

soot in ANSYS Fluent.

Predicting Aerodynamically Generated Noise (p. ), describes the use of the acoustics model in ANSYS

Fluent.

Modeling Discrete Phase (p. ), describes the use of the discrete phase models in ANSYS Fluent.

Modeling Macroscopic Particles (p. ), describes the use of the macroscopic particle models in ANSYS

Fluent.

Modeling Multiphase Flows (p. ), describes the use of the general multiphase models in ANSYS Fluent (VOF,

mixture, and Eulerian).

Population Balance Model (p. ), describes the use of the population balance models in ANSYS Fluent.

Modeling Solidification and Melting (p. ), describes the use of the solidification and melting model in

Modeling Fluid-Structure Interaction (FSI) Within Fluent (p. ), describes the use of a structural model for

intrinsic fluid-structure interaction (FSI) simulations in ANSYS Fluent.

Modeling Eulerian Wall Films (p. ), describes the use of the Eulerian wall film model in ANSYS Fluent.

Modeling Electric Potential Field (p. ), describes the use of the electric potential model in ANSYS Fluent.

Modeling Batteries (p. ), describes the use of the battery models in ANSYS Fluent.

Modeling Fuel Cells (p. ), describes the use of the fuel cell models in ANSYS Fluent.

Modeling Magnetohydrodynamics (p. ), describes the use of the magnetohydrodynamics models in ANSYS

Fluent.

Modeling Continuous Fibers (p. ), describes the use of the continuous fiber model in ANSYS Fluent.

Creating Reduced Order Models (ROMs) (p. ), describes the use of the reduced order model in ANSYS

Fluent.

Using the Solver (p. ), describes the use of the ANSYS Fluent solvers.

Adapting the Mesh (p. ), describes the use of the solution-adaptive mesh refinement feature in ANSYS

Fluent.

Creating Surfaces and Cell Registers for Displaying and Reporting Data (p. ), describes how to create

surfaces in the domain on which you can examine ANSYS Fluent solution data.

Displaying Graphics (p. ), describes the use of the graphics tools to examine your ANSYS Fluent solution.

Reporting Alphanumeric Data (p. ), describes how to obtain reports of fluxes, forces, surface integrals,

and other solution data.

Field Function Definitions (p. ), describes the flow variables that appear in the variable selection drop-

down lists in ANSYS Fluent dialog boxes, and tells you how to create your own custom field functions.

Parallel Processing (p. ), describes the use of the parallel processing features in ANSYS Fluent.This chapter

also provides information about partitioning your mesh for parallel processing.

Design Analysis and Optimization (p. ), describes the use of the adjoint solver and the mesh morpher/op-

timizer.These features allow you to modify the design and solve optimization problems in ANSYS Fluent.

Performing System Coupling Simulations Using Fluent (p. ), describes connecting ANSYS Fluent to external

solvers.

Customizing Fluent (p. ), provides information about using ANSYS ACT to create simulation wizards that

can be run from either stand-alone Fluent or Fluent in Workbench.

Task Page Reference Guide (p. ), describes the use of the task pages within the ANSYS Fluent user interface.

Ribbon Reference Guide (p. ), describes the File ribbon tab and other dialog boxes that are available from

the ribbon at the top of the ANSYS Fluent   user interface.

Appendix A: ANSYS Fluent Model Compatibility (p. ), presents a series of tables outlining the compatibility

of several ANSYS Fluent model categories.

Appendix B: ANSYS Fluent File Formats (p. ), presents information about the contents and formats of

ANSYS Fluent   case, data, and mesh morpher/optimizer files.

Appendix C: Controlling CHEMKIN-CFD Solver Parameters Using Text Commands (p. ), describes the

available text commands that can be used to control or improve the performance and convergence behavior

of the CHEMKIN-CFD solver withinANSYS Fluent, as well as their default values and their recommended use.

Appendix D: Nomenclature (p. ), presents a brief listing of the physical properties and fluid dynamic

quantities used throughout the ANSYS Fluent documentation.

Using This Manual

This preface is divided into the following sections:

.Typographical Conventions

. Mathematical Conventions

Several typographical conventions are used in this manual’s text to help you find commands in the

user interface.

Different type styles are used to indicate graphical user interface items and text interface items. For

example:

Iso-Surface dialog box

surface/iso-surface text command

The text interface type style is also used when illustrating exactly what appears on the screen to distin-

guish it from the narrative text. In this context, user inputs are typically shown in boldface. For example,

solve/initialize/set-fmg-initialization

Customize your FMG initialization:

set the number of multigrid levels []

set FMG parameters on levels ..

residual reduction on level  is:  [.]

number of cycles on level  is:  []

Mini flow charts are used to guide you through the ribbon or the tree, leading you to a specific option,

dialog box, or task page.The following tables list the meaning of each symbol in the mini flow charts.

Table : Mini Flow Chart Symbol Descriptions

Indicated Action

Symbol

Look at the ribbon

Look at the tree

Double-click to open task page

Select from task page

Symbol

Right-click the preceding item

Setting Up Domain → Mesh → Transform → Translate...

dxlv

indicates selecting the Setting Up Domain ribbon tab, clicking Transform (in the Mesh group

box) and selecting Translate..., as indicated in the figure below:

And

Setup → Models → Viscous

Model → Realizable k-epsilon

indicates expanding the Setup and Models branches, right-clicking Viscous, and selecting

Realizable k-epsilon from the Model sub-menu, as shown in the following figure:

And

Setup →

Boundary Conditions →

velocity-inlet-

indicates opening the task page as shown below:

dxlvi

In this manual, mini flow charts usually accompany a description of a dialog box or command,

or a screen illustration showing how to use the dialog box or command. They show you how to

quickly access a command or dialog box without having to search the surrounding material.

In-text references to File ribbon tab selections can be indicated using a “/”. For example

File/Write/Case... indicates clicking the File ribbon tab and selecting Case... from the Write submenu

(which opens the Select File dialog box).

Where possible, vector quantities are displayed with a raised arrow (e.g.,

,

). Boldfaced characters are re-

served for vectors and matrices as they apply to linear algebra (e.g., the identity matrix, ).

The operator

, referred to as grad, nabla, or del, represents the partial derivative of a quantity with respect

to all directions in the chosen coordinate system. In Cartesian coordinates,

is defined to be

()

appears in several ways:

()

– The gradient of a scalar quantity is the vector whose components are the partial derivatives; for example,

()

– The gradient of a vector quantity is a second-order tensor; for example, in Cartesian coordinates,

dxlvii

Mathematical Conventions

()

This tensor is usually written as

()

– The divergence of a vector quantity, which is the inner product between

and a vector; for example,

()

– The operator

, which is usually written as

and is known as the Laplacian; for example,

()

is different from the expression

, which is defined as

()

An exception to the use of

is found in the discussion of Reynolds stresses in Turbulence in the Fluent

Theory Guide, where convention dictates the use of Cartesian tensor notation. In this chapter, you will also

find that some velocity vector components are written as , , and

instead of the conventional  with

directional subscripts.

dxlviii

Chapter : Graphical User Interface (GUI)

The Fluent graphical interface consists of a ribbon (tabs), a toolbar, a tree, a task page, a graphics toolbar,

graphics windows, and a console, which is a textual command line interface (described in Text User

Interface (TUI) (p. )). You will also have access to the dialog boxes via the ribbon or task pages.

.. GUI Components

.. Modifying the Graphical User Interface

.. Fluent Graphical User Interface in Japanese

The graphical user interface (GUI) is made up of seven main components, which are described in detail

in the subsequent sections: the ribbon, the tree, toolbars, task pages, a console, dialog boxes, and

graphics windows. When you use the GUI, you will be interacting with one of these components at all

times. The GUI will change depending on whether you are in meshing mode (as described in the Fluent

Meshing section of the User’s Guide) or solution mode (as described in this guide, and as shown in

Figure . : The GUI Components (p. )). For details on how to switch between these modes, see

Switching Between Meshing and Solution Modes (p. ) in the Getting Started Guide.

Many of the GUI elements can be moved or tabbed together to suit your preferences. You can also

modify attributes of the GUI to better match your platform environment. These are described in Modi-

fying the Graphical User Interface (p. ) and Setting User Preferences/Options (p. ).

Figure . : The GUI Components

...The Outline View

... Graphics Windows

...Toolbars

...Task Pages

... Dialog Boxes

The ribbon, located at the top of the Fluent GUI, is the primary method for setting up and running

your simulation. It facilitates access to the most commonly used items, with tabs nominally arranged

in a left to right workflow for a typical simulation. Contents within each tab are grouped with related

content and are organized logically to accommodate varied projects and priorities. You have the option

to minimize the ribbon by clicking

, located to the right of the ribbon tabs.

Figure . : The Fluent Ribbon

Graphical User Interface (GUI)

Often, making a selection in the ribbon opens a dialog box. In some instances, a ribbon selection opens

a task page.

The outline view tree, located on the left side of the Fluent GUI, is an interactive representation of

your project. Its items are listed in an order that complements the typical problem setup you follow

in the ribbon. Branches can be expanded and collapsed to suit your preferences.

You can select multiple related items by left-clicking and dragging or using Shift/Ctrl + left-click. Right-

clicking selected items in the tree provides a list of common commands. Typographical Conven-

tions (p. dxlv) shows the convention used to describe this right-click action, when it is referred to in the

documentation.

Figure . : The Fluent Outline View

You can perform wildcard and regular expression searches in the tree using the filter text entry box

at the top of the tree; see Filter Text Entry Boxes (p. ) for additional information.

Double-clicking many of the branches under Setup, Solution, or Results displays the corresponding

Task Page to the right of the tree. For additional information, see (Task Pages (p. )).

GUI Components

Drag and Drop, Copy and Paste

There are multiple uses for drag and drop operations with a running Fluent session. You can use drag

and drop to:

Open files by dropping them onto the open Fluent session.

The supported file types include:

– Case and data (*.cas, *.cas.gz, *.dat, *.dat.gz, *.msh, *.msh.gz)

– Journals (*.jou, *.log)

– Profiles (*.csv)

– PDFs (*.pdf)

Copy various settings and objects within a Fluent session and across Fluent sessions. For example, you can

drag a report definition from one session and drop it on another open Fluent session.This report definition

will then be created in the new session. Note that Fluent displays a plus ( ) icon for valid drop operations and

a invalid (

) icon for operations or locations that are not allowed.

Display items in the graphics window by dragging them from the tree and dropping them on the graphics

window.This functions like the Add to graphics right-click option.

Copy and paste is available for copying items from the outline view to the clipboard so that you can

paste them elsewhere in the same session or into another session without having to hold down the

left-mouse-button like you do for a drag and drop operation. Copy and paste is available for:

Boundary conditions

Named expressions

Report definitions, files, and plots

Postprocessing objects (mesh, contours, and so on)

Export To File and Import From File

Export To File... and Import From File... are available as right-click options for certain branches in

the outline view, including:

Report definitions

Postprocessing objects

These options allow you to save the settings of a single sub-branch (for example, a single boundary

condition or named expression) or all of the items in the higher-level branch (for example, all of the

boundaries or all of the named expressions) for later use. These exports are saved in .tsv format.

Graphics windows display the program’s graphical output, and may be viewed within the Fluent ap-

plication window or in separate windows. You can right-click the top of the graphics window to select

whether you want new graphics windows to be tabbed or as additional sub-windows within the

graphics window group space. By default, graphics windows viewed within the application window

will be placed below the toolbar on the right, as shown in Figure . : The GUI Components (p. ).

Using context menus in the graphics window you can access and modify settings directly on the

model. Figure . : Graphics Window Context Menu: Single-Selection (p. ) and Figure . : Graphics

Window Context Menu: Multiple-Selection (p. ) demonstrate some of the options available via right-

click. You can make multiple selections on the displayed graphics object by holding Ctrl.

Figure . : Graphics Window Context Menu: Single-Selection

Figure . : Graphics Window Context Menu: Single-Selection (p. ) shows right-clicking the inlet (selection

highlighted in green) and specifying it as a pressure-inlet.

Figure . : Graphics Window Context Menu: Multiple-Selection

Figure . : Graphics Window Context Menu: Multiple-Selection (p. ) shows right-clicking the object when

multiple surfaces are selected and a scene is displayed.

Note

There are a few situations where a right-click in the graphics window will not open a context

menu:

Right-mouse-button (RMB) is set as mouse-probe and you right-click on the model when

nothing is selected.

RMB is set as mouse-probe and long description and you right-click anywhere in the graphics

window when nothing is selected.

RMB is set as mouse-zoom.

For additional information on mouse button settings, see Controlling the Mouse Button

Functions (p. ).

In Figure . : Displaying Two Graphics Windows (p. ), two graphics windows are displayed by right-

clicking the top of the graphics window and selecting SubWindow View, then creating two graphical

displays and fitting them in the space accordingly.

Figure . : Displaying Two Graphics Windows

The Display Options dialog box (see Display Options Dialog Box (p. )) can be used to change the

attributes of the graphics window or to open another graphics window. In the View tab (Mouse group

box), you can set the action taken in the graphics window when a mouse button is pressed (see

Modifying the Mouse Button Functions (p. ) for details).

Important

To cancel a display operation, press Ctrl+c while the data is being processed in preparation

for graphical display. You cannot cancel the operation after the program begins to draw in

Important

It is possible that the graphics window may become [Out of Date] (which would be indicated

at the top of the graphics window), if you make changes to items that are already displayed.

To resolve this out of date state, right-click in the graphics window and click Refresh Display

in the context menu that appears.

If a context menu does not appear on a right-click of the graphics window, ensure that the right-

mouse button is set to an action other than mouse-zoom or mouse-probe and long description

(View ribbon tab, Mouse group box).

Copy to Clipboard

Right-clicking the graphics window tab allows you to select Copy to Clipboard. This places a copy of

the current picture displayed in the selected graphics window tab onto your clipboard. The size of

your graphics window affects the size of the text fonts used in the picture.

The search bar (upper right of the Fluent window or via Ctrl + F) allows you to quickly locate the

commands or controls that you are looking for. Clicking the search results is equivalent to clicking the

same control in the ribbon. Hovering over a search result highlights the location of the control in the

ribbon. Clicking a text command search result automatically enters the text of the command, but it

does not execute the command; you still have to press Enter in the console to execute the text com-

mand.

The Fluent GUI includes toolbars located within the application window. These toolbars provide

shortcuts to performing common tasks in Fluent. The toolbars include a standard toolbar and an objects

toolbar.

....The Standard Toolbar

The standard toolbar (Figure . : The Standard Toolbar (p. )) contains options for getting help, ar-

ranging the graphical user interface, and visiting the ANSYS website.

Figure . : The Standard Toolbar

The following is a brief description of each of the standard toolbar options:

Help

allows you to access the Fluent User's Guide (p. ) for help topics. For more information, see

Using the Help System (p. ).

Arrange the workspace

provides you with several application window layout options. For example,

you can choose to hide certain windows or have the graphics window be much larger than the other

elements.These options also allow you to return to a standard layout if you accidentally rearrange (by

dragging and dropping, or closing elements) the workspace in an undesirable manner.

Link to the ANSYS Website

opens a link to the ANSYS home page in your default browser.

....The Graphics Toolbar

Figure . : The Graphics Toolbar

The following tools are available in the graphics toolbar:

..... Pointer Tools

.....View Tools

..... Projection Tools

..... Mesh Display Configuration

..... Additional Display Options

The pointer tools (Figure . : The Pointer Tools (p. )) allow you to modify the way in which you

view your model or select objects in the graphics window.

Figure . : The Pointer Tools

The following is a description of each of the pointer tools:

lets you rotate your model about a central point in the graphics window. For more

information, see Button Functions (p. ).

Pan

allows you to pan horizontally or vertically across the view using the left mouse button. For

more information, see Button Functions (p. ).

allows you to zoom in to and out of the model by holding the left mouse button

down and moving the mouse down or up. For more information, see Button Functions (p. ).You can

also roll the view by holding the left mouse button down and moving the mouse left or right.

allows you to focus on any part of your model. After selecting this option, position

the mouse pointer at a corner of the area to be magnified, hold down the left mouse button and drag

open a box to the desired size, and then release the mouse button.The enclosed area will then fill the

graphics window. Note that you must drag the mouse to the right in order to zoom in.To zoom out, you

must drag the mouse to the left. For more information, see Button Functions (p. ).

Print information about selected item

allows you to select items from the graphics windows and

request information about displayed scenes.This behaves as a mouse probe button. For more information,

see Button Functions (p. ).

The view tools (Figure . : The View Tools (p. )) allow you to modify the way your model is dis-

played in the graphics window.

Figure . : The View Tools

The following is a description of each of the view tools:

Last View

allows you to revert to the displayed objects previous location and orientation in the

Set view

contains a drop-down of views, allowing you to display the model from the direction of

the vector equidistant to all three axes, as well as in different axes orientations.

allows you to capture an image of the active graphics window. For more information,

see Saving Picture Files (p. ).

The projection tools (Figure . : The Projection Tools (p. )) allow you to modify the perspective

of objects in the graphics window.

Figure . : The Projection Tools

The following is a brief description of each of the projection tools:

Perspective View

shows the 3D object on your 2D screen approximately how your eye would see

it in real life.This button is only available when running Fluent in 3D.

Orthographic View

shows 3D objects to scale, ignoring perspective view. When enabled, it makes

it so the ruler is accurate.This button is only available when running Fluent in 3D.

Note

When Orthographic is selected for Graphics view in Preferences (Appearance branch),

an additional Ruler option appears. Enabling Ruler makes it so that the ruler is displayed

whenever the view is changed to orthographic. You can still disable the ruler by toggling

the ruler button

).

The mesh display configuration options (Figure . : Mesh Display Configuration (p. )) contains

predefined settings for how a mesh and objects are displayed.

Figure . : Mesh Display Configuration

The following is a brief description of the configuration options:

Mesh Display Configuration

contains options for changing how the mesh displays in the graphics window.

– Meshing

draws mesh on edges and faces of the outline surfaces, colored by their zone ID with lighting

enabled.

– Solution

draws mesh on edges and faces of the outline surfaces, colored by their zone type with lighting

enabled.

– Post Processing

draws the object outline with lighting disabled.

– Classic

draws mesh on all edges of the outline surfaces.

The additional display options (Figure . : Additional Display Options (p. )) provides access to

– Classic

the Mesh Display Dialog Box (p. ) and the ability to make the outer faces transparent.

Figure . : Additional Display Options

The following is a description of each of the additional display options:

Ruler Visibility

turns the ruler on and off.When enabled, it switches the view to orthographic (if

it was previously set to perspective).

Mesh Display

opens the Mesh Display Dialog Box (p. ).

makes the front faces of the displayed object transparent, allowing you

to see inside.

turns the titles display on and off.

copies the current picture displayed in the selected graphics window tab onto

your clipboard.

Task pages appear on the right side of the tree when certain branches are double-clicked. They provide

access to more advanced settings than are often available through a right-click of the same branch or

sub-branches. The expected workflow is that you travel down the tree, using a right-click most branches

and sub-branches to access the settings and controls required for to solve your problem.

Some of your setup will occur in dialog boxes, while others in task pages. For example, if you double-

click General in the tree, the General Task Page (p. ) is displayed. Global settings are made in this

task page, which are saved to the case definition.

Each task page has a Help button. Clicking this button opens the related help topic in the Task Page

Reference Guide (p. ). See Using the Help System (p. ) for more information.

The console is located below the graphics window, as shown in Figure . : The GUI Components (p. ).

Fluent communicates with you through the console. It is used to display various kinds of information

(that is, messages relating to meshing or solution procedures, and so on). Console text is colored based

on whether it is user-input, standard output, or a warning message. Fluent saves a certain amount of

information that is written to the console into memory. You can review this information at any time

by using the scroll bar on the right side of the console. You can enable/disable autoscrolling using the

check box at the bottom right of the console to either have the cursor jump to the latest printed

content or stay where it is. The size of the console can be adjusted by raising or lowering the bottom

frame of the graphics window.

The console is similar in behavior to “xterm” or other Linux command shell tools, or to the MS-DOS

Command Prompt window on Windows systems. It allows you to interact with the TUI menu. More

information on the TUI can be found in Text User Interface (TUI) (p. ).

The console accepts a “break” command (pressing Ctrl+c at the same time) to let you interrupt the

program while it is working. It also lets you perform text copy and paste operations between the

console and other X Window (or Windows) applications that support copy and paste. The following

steps show you how to perform a copy and paste operation on a Windows system:

. Move the pointer to the beginning of the text to be copied.

. Press and hold down the left mouse button.

. Move the pointer to the end of the text (text should be highlighted).

. Release the left mouse button.

. Press the Ctrl and <Insert> keys at the same time.

. Move the pointer to the target window and click the left mouse button.

. Press the Ctrl+v keys at the same time.

On a Linux system, you will follow the steps below to copy text to the clipboard:

Note

The console has a , line retention limit. Once the number of lines passes ,, the

auto-scroll checkbox (lower right of the Console) no longer has an effect.

There are two types of dialog boxes in Fluent. Some dialog boxes are used to perform simple input/out-

put tasks, such as issuing warning and error messages, or asking a question requiring a yes or no answer.

Other forms of dialog boxes allow you to perform more complicated input tasks.

A dialog box is a separate “temporary” window that appears when Fluent needs to communicate with

you, or when various types of input controls are employed to set up your case. The types of controls

you will see are described further in this section.

When you have finished entering data in a dialog box’s controls, you must apply the changes you

have made, or cancel the changes, if desired. For this task, each dialog box falls into one of two beha-

vioral categories, depending on how it was designed.

The first category of dialog boxes is used in situations where it is desirable to apply the changes and

immediately close the dialog box. This type of dialog box includes an OK and a Cancel button that

function as described below:

OK

applies any changes you have made to the dialog box, then closes the dialog box.

Cancel

closes the dialog box, ignoring any changes you have made.

An example of this type of dialog box is shown in the following figure:

The other category of dialog boxes is used in situations where it is desirable to keep the dialog box

displayed on the screen after changes have been applied. This makes it easy to quickly go back to that

dialog box and make more changes. Dialog boxes used for postprocessing and mesh adaption often

fall into this category. This type of dialog box typically includes an Apply button and a Close button

as described below:

Apply

applies any changes you have made to the dialog box, but does not close the dialog box.The name of

this button is often changed to something more descriptive. For example, many of the postprocessing

dialog boxes use the name Display for this button, and the adaption dialog boxes use the name Adapt.

Close

closes the dialog box.

All dialog boxes include the following button used to access ANSYS Help:

Help

Close

Help

displays information about the controls in the dialog box.The information appears in the ANSYS Help

Viewer.

Many dialog boxes also present additional buttons to accomplish specific tasks or open additional

dialog boxes. You can find descriptions of the functions of these additional buttons in Ribbon Reference

Guide (p. ) or Task Page Reference Guide (p. ).

Note

Dialog boxes containing lists are expandable.

.... Input Controls

Each type of input control utilized by the dialog boxes is described below. Note that the examples

shown here are for a Windows system; if you are working on a Linux system, your dialog box controls

may look slightly different, but they will work exactly as described here.

.....Tabs

Much like the tabs on a notebook divider, tabs in dialog boxes are used to mark the different sections

into which a dialog box is divided. A dialog box that contains many controls may be divided into

different sections to reduce the amount of screen space it occupies. You can access each section of

the dialog box by “clicking” the left mouse button on the corresponding tab. A click is one press

and release of the mouse button.

..... Buttons

A button, also referred to as a push button, is used to perform a function indicated by the button

label. To activate a button, place the pointer over the button and click the left mouse button.

..... Check Boxes

A check box, also referred to as a check button, is used to enable / disable an item or action indicated

by the check box label. Click the left mouse button on the check box to toggle the state.

..... Radio Buttons

Radio buttons are a set of check boxes with the condition that only one can be set in the “on” pos-

ition at a time. When you click the left mouse button on a radio button, it will be turned on, and all

others will be turned off. Radio buttons appear either as diamonds (in Linux systems) or as circles

(as shown above).

.....Text Entry Boxes

A text entry box lets you type text input. It will often have a label associated with it to indicate the

purpose of the entry.

..... Integer Number Entry Boxes

An integer number entry box is similar to a text entry except it only allows integer numbers to be

entered (for example, , -,  and 5E4). You may find it easier to enter large integer numbers

using scientific notation. For example, you could enter  or .5E5.

The integer number entry also has arrow buttons that allow you to easily increase or decrease its

value. For most integer number entry controls, the value will be increased (or decreased) by one

when you click an arrow button. You can increase the size of the increment by holding down a

keyboard key while clicking the arrow button. The keys used are shown below:

Factor of Increase

Key

Shift

Ctrl

..... Real Number Entry Boxes

A real number entry box is similar to a text entry, except it only allows real numbers to be entered

(for example, , -., . and .72E-). In most cases, the label will show the units associated

with the real number entry.

..... Filter Text Entry Boxes

The filter text entry box allows you to search and organize a list using a text string. The text string

can include wildcards and regular expressions, which allow you to perform pattern matching. For

example, searching *let* finds surfaces such as inlets and outlets, including those with longer

names, such as "upper-inlet-". If you have walls separated by a number, you can search example-

wall-?-, which would show example-wall--, example-wall--, and so on.

Filtering begins as soon as you enter text. Clicking Enter expands any sub-branches containing

matches to the entered string.

..... Single-Selection Lists

A single-selection list presents a list of items, with each item printed on a separate line. You can

select an item by placing the pointer over the item line and clicking with the left mouse button. The

selected item will become highlighted. Selecting another item will deselect the previously selected

item in the list.

Many dialog boxes will also accept a double-click in order to invoke the dialog box action that is

associated with the list selection (see information on the dialog box of interest for more details).

..... Multiple-Selection Lists

A multiple-selection list is similar to a single-selection list, except it allows for more than one selected

item at a time. When you click the left mouse button on an item, its selection state will toggle.

Clicking an unselected item will select it. Clicking a selected item will deselect it.

To select a range of items in a multiple-selection list, you can select the first desired item, and then

select the last desired item while holding down the Shift key. The first and last items, and all the

items between them, will be selected. You can also click and drag the left mouse button to select

multiple items.

There are several small buttons in the upper right corner of the multiple selection list to accelerate

selecting or deselecting items from the selection list.

Click

to display all of the items that are currently selected.

Click

or

to toggle to a tree view of the selection list, and thereby group items by categories

such as name or surface type. You can select or deselect all the items in a particular group by

clicking the top-level branch. For example, if you have the surfaces grouped by Surface Type,

clicking Inlet will select or deselect all inlets. Note that once you switch to a tree view, the icon

changes to

or

, respectively.

Click

to select all the items displayed in the selection list.

Click

to deselect all the items displayed in the selection list.

..... Drop-Down Lists

A drop-down list is a hidden single-selection list that shows only the current selection to save space.

When you want to change the selection, follow the steps below:

. Click the arrow button to display the list.

. Place the pointer over the new list item.

. Click the left mouse button on the item to make the selection and close the list.

If you want to stop the selection operation while the list is displayed, you can move the pointer

anywhere outside the list and click the left mouse button.

..... Scales

A scale is used to select a value from a predefined range by moving a slider. The number shows the

current value. You can change the value by clicking the arrow buttons, or by following one of the

procedures below:

. Place the pointer over the slider.

. Move the pointer along the slider bar to change the value.

or

. Place the pointer over the slider and click the left mouse button.

. Using the arrow keys on the keyboard, move the slider bar left or right to change the value.

....Types of Dialog Boxes

The following sections describe the various types of dialog boxes.

..... Information Dialog Boxes

The Information dialog box is used to report some information that Fluent thinks you should know.

After you have read the information, you can click the OK button to close the dialog box.

.....Warning Dialog Boxes

The Warning dialog box is used to warn you of a potential problem or deliver an important message.

Your control of Fluent will be suspended until you acknowledge the warning by clicking the OK

button.

..... Error Dialog Boxes

The Error dialog box is used to alert you of an error that has occurred. After you have read the error

information, you can click the OK button to close the dialog box.

.....The Working Dialog Box

The Working dialog box is displayed when Fluent is busy performing a task. This is a special dialog

box, because it requires no action by you. It is there to let you know that you must wait. When the

program is finished, it will close the dialog box automatically. You can, however, abort the task that

is being performed by clicking the Cancel button.

..... Question Dialog Box

The Question dialog box is used to ask you a question. Sometimes the question will require a Yes

or No answer, while other times it will require that you either allow an action to proceed (OK) or

Cancel the action. You can click the appropriate button to answer the question.

.....The Select File Dialog Box

File selection is accomplished using the Select File dialog box (The Select File Dialog Box (Win-

dows) (p. ) or The Select File Dialog Box (Linux) (p. )).

......The Select File Dialog Box (Windows)

File selection on Windows systems is accomplished using the standard Windows Select File dialog

box (Figure . : The Select File Dialog Box for Windows (p. )).

Figure . : The Select File Dialog Box for Windows

See documentation regarding your Windows system for further instructions on file selection.

Note

If you are accessing a file using a Universal Naming Convention (UNC) path, you must

ensure that you have permission to access to all of the folders in the path or you will not

be able to open the file.

......The Select File Dialog Box (Linux)

For Linux systems, note that the appearance of the Select File dialog box will not always be the

same.

The version shown in Figure . : The Select File Dialog Box for Linux Platforms (p. ) will appear

in almost all cases, but it will be different if you are loading external data files for use in an XY plot

(see Including External Data in the Solution XY Plot (p. ) for more information). In such cases, the

dialog box will look like Figure . : Another Version of the Select File Dialog Box for Linux Plat-

forms (p. ).

Figure . : The Select File Dialog Box for Linux Platforms

Figure . : Another Version of the Select File Dialog Box for Linux Platforms

The steps for file selection are as follows:

. Go to the appropriate directory.You can do this in two different ways:

Enter the path to the desired directory in the Filter text entry box and then press the Enter key or

click the Filter button. Be sure to include the final / character in the pathname, before the optional

search pattern (described below).

Double-click a directory, and then a subdirectory, and so on, in the Directories list until you reach

the directory you want.You can also click once on a directory and then click the Filter button, instead

of double-clicking. Note that the “ .” item represents the current directory and the “ ..” item represents

the parent directory.

Note

ensure that you have permission to access to all of the folders in the path or you will

not be able to open the file.

. Specify the file name by selecting it in the Files list or entering it in the File text entry box (if available)

at the bottom of the dialog box.The name of this text entry box will change depending on the type of

file you are selecting (Case File, Journal File, and so on).

Important

Note that if you are searching for an existing file with a nonstandard extension, you

may need to modify the “search pattern” at the end of the path in the Filter text entry

Important

box. For example, if you are reading a data file, the default extension in the search

path will be *.dat*, and only those files that have a .dat extension will appear in

the Files list. If you want files with a .DAT extension to appear in the Files list, you

can change the search pattern to *.DAT*. If you want all files in the directory to be

listed in the Files list, enter just * as the search pattern.

. If you are reading a mesh or case file, use the Display Mesh after Reading option to specify whether

you want Fluent to automatically display the mesh after the file is read. All of the boundary zones will

be displayed, except for the interior zones of 3D geometries.The default status of this option (that is,

enabled or disabled) is determined by your decision regarding the Display Mesh After Reading option

in Fluent Launcher.

. If you are using the Replace Mesh... option in the  Domain tab (Zones group box) to replace a mesh

with existing data, you can enable the Interpolate Data Across Zones option to interpolate the data

across cell zones.This option is appropriate when the matching zone pairs (that is, the zones with the

same names in both the current mesh and the replacement mesh) do not have the same interior zone

boundaries. See Replacing the Mesh (p. ) for details.

. If you are reading multiple XY-plot data files, the selected file will be added to the list of XY File(s).You

can choose another file, following the instructions above, and it will also be added to this list. (If you

accidentally select the wrong file, you can choose it in the XY File(s) list and click the Remove button

to remove it from the list of files to be read.) Repeat until all of the desired files are in the XY File(s) list.

. If you are writing a case, data, or radiation file, use the Write Binary Files check box to specify whether

the file should be written as a text or binary file.You can read and edit a text file, but it will require more

storage space than the same file in binary format. Binary files take up less space and can be read and

written by Fluent more quickly.

. Click the OK button to read or write the specified file. Shortcuts for this step are as follows:

If your file appears in the Files list and you are not reading an XY file, double-click it instead of just

selecting it.This will automatically activate the OK button. (If you are reading an XY file, you will always

have to click OK yourself. Clicking or double-clicking will just add the selected file to the XY File(s)

list.)

If you entered the name of the file in the File text entry box, you can press the Enter key instead of

clicking the OK button.

are arranged and sized. This can be achieved by “dragging” elements and “dropping” them at a new

location and by grabbing near the edge and expanding or collapsing the selected element. For example,

certain items can be tabbed on top of other items, such as the graphics window on top of the console.

The items that you can move include the console, the task page, and the toolbars. You can resize these

elements while the solver is calculating to adjust the focus towards your area of interest, such as increas-

ing the size of the graphics window.

To restore items that you intentionally or unintentionally closed, click

in the upper-right of the

Fluent window, to select one of the predefined layouts and restore missing items. You can also right-

click the top portion of the Outline View or Console to restore missing items.

You may want to customize the graphical user interface by changing attributes such as text color,

background color, and text fonts. You can control many of these settings globally, using Preferences

(see Setting User Preferences/Options (p. ) for more information). The program will try to provide

default text fonts that are satisfactory for your platform’s display size, but in some cases customization

may be necessary if the default text fonts make the GUI too small or too large on your display, or if the

default colors are undesirable.

Tooltips are available when you hover over setting labels that clarify the purpose/function of the setting.

Note

session.

If you change a setting locally that is also controlled by Preferences, the local change will be

shown for this session only. If you open the Preferences dialog box and click Apply in an attempt

to overwrite the local settings change, the global setting will only appear if it is a change from

how the setting is already specified globally. For example, if you have ANSYS Logo set as Black

in Preferences, then you change the logo to White in the Display Options dialog box, the logo

will change from black to white. If you then re-open the Preferences dialog box and click Apply,

the logo will remain white, even though it is specified as Black in the preferences dialog box.

The reason being that globally, the logo is already specified as black, so clicking Apply does not

change the current global color of the logo, which is being overruled by your local change to

white.

The controlling preferences file location is:

white.

Windows: %HOMEDRIVE%\%HOMEPATH%\.fluentconf\..\preferences

Linux: %HOMEPATH%/.fluentconf/../preferences

If no preference file is found (for instance, after installation of a new version or deletion of the preference

file), Fluent will attempt to load user preferences from a previous version. If no previous version's preferences

are found, Fluent will create a new file using the default settings.

At any time, you can revert your preferences to the default settings by clicking the Default button in the

Preferences dialog box. Or you can delete the preferences file and Fluent will follow the above rule to create

a new one.

You can have the Fluent graphical user interface appear in Japanese by defining the lang=ja environ-

ment variable before launching Fluent (you can define it in the Environment tab of the Fluent

Launcher).

Figure . : Fluent GUI in Japanese

Limitations for Localization

Some areas of the Fluent  R3 GUI are not translated into Japanese including:

Drop-down menu/list items

Quick search results

Pop up messages

Graphics window titles and labels

Object names (boundary conditions, graphics objects, and so on)

Fluent Graphical User Interface in Japanese

The Outline View tree in meshing mode

Interface (GUI labels) for items without a meaningful Japanese equivalent, for example X,Y, Z, Cp, OK, and

so on

You can access documentation, videos, and tutorials on the ANSYS Help site.

Fluent includes an integrated help system that provides easy access to the program documentation.

Through the graphical user interface, you have the entire User's Guide (p. ) and other documentation

available to you with the click of a mouse button. The Fluent User's Guide and other manuals are dis-

played on the ANSYS help site, which allows you to use links and search tools and index tools to find

the information you need.

There are many ways to access ANSYS help. You can get reference information from within a task page

or dialog box, or (on Linux machines) request context-sensitive help for a particular task page item or

dialog box. You can also go to the User's Guide (p. ) contents page and use the links to find the in-

formation you are looking for. In addition to the User's Guide (p. ), you can also access the other

Fluent documentation (for example, the Theory Guide or Fluent Customization Manual).

Note that the last two chapters of the User's Guide (Task Page Reference Guide (p. ) and Ribbon

Reference Guide (p. )) (p. ) are also referred to as the Reference Guide, and contain a description

of each task page, and dialog box.

The sections that follow provide information on how to get help for a task page or dialog box, and

brief descriptions of the help menu items in Fluent.

...Task Page and Dialog Box Help

... Context-Sensitive Help (Linux Only)

... Obtaining License Use Information

...Version and Release Information

To get help about a task page or dialog box that you are currently using, click the Help button in the

task page or dialog box. The help will open to the section of the User's Guide (p. ) that explains the

function of each item in the task page or dialog box. In this section, you will also find hypertext links

to more specific section(s) of the User's Guide (p. ) that discuss how to use the task page or dialog

box and provide related information.

If you want to find out how or when a particular task page item or dialog box is used, you can use

the context-sensitive help feature. Select the Context-Sensitive Help item in the help menu (accessed

by clicking

).

With the resulting question-mark cursor, select an item from a drop-down menu. The help will open

to the section of the User's Guide (p. ) that discusses the selected item.

Your installation of Fluent is managed by the ANSYS License Manager (ANSLIC_ADMIN). To learn more

about ANSYS licensing information, refer to the ANSYS, Inc. Licensing Guide.

You can obtain information about the version and release of Fluent you are running by selecting the

Version... option in help menu (accessed by clicking

).

Chapter :Text User Interface (TUI)

During an ANSYS Fluent session you may need to import and export several kinds of files. Files that are

read include mesh, case, data, profile, Scheme, and journal files. Files that are written include case, data,

profile, journal, and transcript files. ANSYS Fluent also has features that enable you to save pictures of

graphics windows. You can also export data for use with various visualization and postprocessing tools.

These operations are described in the following sections.

.. Reading Mesh Files

.. Reading and Writing Case and Data Files

.. Reading Fluent/UNS and RAMPANT Case and Data Files

.. Reading and Writing Profile Files

.. Reading and Writing Boundary Conditions

..Writing a Boundary Mesh

.. Exporting Solution Data

.. Exporting Solution Data after a Calculation

.. Exporting Steady-State Particle History Data

.. Exporting Data During a Transient Calculation

.. Exporting to ANSYS CFD-Post

.. Parallel Exporting to ANSYS EnSight

.. Managing Solution Files

.. Mesh-to-Mesh Solution Interpolation

.. Mapping Data for Fluid-Structure Interaction (FSI) Applications

.. Setting Data File Quantities

..The .fluent File

The following features in ANSYS Fluent make reading and writing files convenient:

Automatic appending or detection of default file name suffixes

Binary file reading and writing

Automatic detection of file format (text/binary)

Recent file list

Reading and writing of compressed files

Tilde expansion

Automatic numbering of files

Ability to disable the overwrite confirmation prompt

Standard toolbar buttons for reading and writing files

... Default File Suffixes

... Detecting File Format

... Recent File List

...Tilde Expansion (Linux Systems Only)

... Automatic Numbering of Files

...Toolbar Buttons

Each type of file read or written in ANSYS Fluent has a default file suffix associated with it. When you

specify the first part of the file name (the prefix) for the commonly used files, Fluent automatically

appends or detects the appropriate suffix. For example, to write a case file named myfile.cas, just

specify the prefix myfile in the Select File dialog box (Figure . : The Select File Dialog Box (p. ))

and .cas is automatically appended. Similarly, to read the case file named myfile.cas into Fluent,

you can just specify myfile and ANSYS Fluent automatically searches for a file of that name with the

suffix .cas.

Figure . : The Select File Dialog Box

The default file suffix for case and data files, PDF (Probability Density Function) files, DTRM ray files,

profiles, scheme files, journal files, and so on, are automatically detected and appended. The appropriate

default file suffix appears in the Select File dialog box for each type of file.

When you write a case, data, or ray file, a binary file is saved by default. Binary files take up less memory

than text files and can be read and written by ANSYS Fluent more quickly.

Note

You cannot read and edit a binary file, as you can do for a text file.

To save a text file, turn off the Write Binary Files option in the Select File dialog box when you are

writing the file. Note that if you use the HDF file format to write out your case and data files, they will

always be binary (Reading and Writing Files Using Hierarchical Data Format (HDF) (p. )).

When you read a case, data, mesh, PDF, or ray file, Fluent automatically determines whether it is a text

(formatted) or binary file.

At the bottom of the File/Read ribbon tab submenu there is a list of four ANSYS Fluent case files that

you most recently read or wrote. To read one of these files into ANSYS Fluent, select it in the list. This

allows you to read a recently used file without selecting it in the Select File dialog box. If you want

to change the number of recent files listed, you can change the Number of files recently used setting

in the Preferences dialog box, which you can access by selecting Preferences... from the File ribbon

tab.

Note that the files listed in this submenu may not be appropriate for your current session (for example,

a 3D case file can be listed even if you are running a 2D version of ANSYS Fluent). Also, if you read a

case file using this shortcut, the corresponding data file is read only if it has the same base name as

the case file (for example, file1.cas and file1.dat) and it was read/written with the case file

the last time the case file was read/written.

You can use the Select File dialog box to read files compressed using compress or gzip. If you

select a compressed file with a .Z extension, ANSYS Fluent automatically opens zcat to import the

file. If you select a compressed file with a .gz extension, Fluent opens gunzip to import the file.

Shortcuts for Reading and Writing Files

For example, if you select a file named flow.msh.gz, Fluent reports the following message indicating

that the result of the gunzip is imported into ANSYS Fluent via an operating system pipe.

Reading "\"| gunzip -c \"Y:\flow.msh.gz\"\""...

You can also type in the file name without any suffix (for example, if you are not sure whether or not

the file is compressed). First, Fluent attempts to open a file with the input name. If it cannot find a

file with that name, it attempts to locate files with default suffixes and extensions appended to the

name.

name.

For example, if you enter the name file-name, Fluent traverses the following list until it finds an

existing file:

file-name

file-name.Z

file-name. suffix

file-name. suffix .gz

file-name. suffix .Z

where suffix is a common extension to the file, such as .cas or .msh. Fluent reports an error if it

fails to find an existing file with one of these names.

Note

In addition to .gz and .Z compression, ANSYS Fluent can also handle .bz2 compressed

files.

Important

For Windows systems, only files that were compressed with gzip (that is, files with a .gz ex-

tension) can be read. Files that were compressed with compress cannot be read into ANSYS

Do not read a compressed ray file; ANSYS Fluent cannot access the ray tracing information

properly from a compressed ray file.

You can use the Select File dialog box to write a compressed file by appending a .Z or .gz extension

onto the file name.

For example, if you enter flow.gz as the name for a case file, Fluent reports the following message:

Writing "| gzip -cfv > Y:\flow.cas.gz"...

The status message indicates that the case file information is being piped into the gzip command,

name. In this particular example, the .cas extension is added automatically.

Note

files.

Important

For Windows systems, compression can be performed only with gzip.That is, you can write

Note

files.

Important

a compressed file by appending .gz to the name, but appending .Z does not compress the

file.

Do not write a compressed ray file; ANSYS Fluent cannot access the ray tracing information

On Linux systems, if you specify ~/ as the first two characters of a file name, the ~ is expanded as

expanded to the home directory of “username”. If you specify ~/file as the case file to be written,

ANSYS Fluent saves the file file.cas in your home directory. You can specify a subdirectory of your

home directory as well: if you enter ~/cases/file.cas, ANSYS Fluent saves the file file.cas in

the cases subdirectory.

There are several special characters that you can include in a file name. Using one of these character

strings in your file name provides a shortcut for numbering the files based on various parameters (that

is, iteration number, time step, or total number of files saved so far), because you need not enter a

new file name each time you save a file. (See also Automatic Saving of Case and Data Files (p. ) for

information about saving and numbering case and data files automatically.)

For transient calculations, you can save files with names that reflect the time step at which they are saved

by including the character string %t in the file name. For example, you can specify contours-%t.ps for

the file name, and Fluent saves a file with the appropriate name (for example, contours-.ps if

the solution is at the first time step).

This automatic saving of files with the time step should not be used for steady-state cases, since

the time step will always remain zero.

For transient calculations, you can save files with names that reflect the flow-time at which they are saved

by including the character string %f in the file name.The usage is similar to %t. For example, when you

specify filename-%f.ps for the file name, Fluent will save a file with the appropriate name (for example,

filename-..ps for a solution at a flow-time of  seconds). By default, the flow-time that

is included in the file name will have a field width of  and  decimal places.To modify this format, use

the character string % x . y f, where x and y are the preferred field width and number of decimal places,

respectively. ANSYS Fluent will automatically add zeros to the beginning of the flow-time to achieve the

prescribed field width.To eliminate these zeros and left align the flow-time, use the character string %- x

. y f instead.

This automatic saving of files with flow-time should not be used for steady-state cases, since the

flow-time will always remain zero.

To save a file with a name that reflects the iteration at which it is saved, use the character string %i in the

file name. For example, you can specify contours-%i.ps for the file name, and Fluent saves a file with

the appropriate name (for example, contours-.ps if the solution is at the 10th iteration).

To save a picture file with a name that reflects the total number of picture files saved so far in the current

Fluent session, use the character string %n in the file name.This option can be used only for picture files.

The default field width for %i, %t, and %n formats is . You can change the field width by using % x

i, % x t, and % x n in the file name, where x is the preferred field width.

it will ask you to confirm that it is “OK to overwrite” the existing file. If you do not want Fluent to ask

you for confirmation before it overwrites existing files, you can use the Batch Options dialog box (see

Batch Execution Options (p. ) in the Getting Started Guide for details). Alternatively, enter the

file/confirm-overwrite? text command and answer no (see Text User Interface (TUI) (p. )

for the text user interface commands).

The standard toolbar provides buttons that make it easier to read and write files:

The Read a file button (

) allows you to read existing files using a file selection dialog box.The files

available for reading include all those available through the File/Read ribbon tab item, as described in this

chapter.

The Write a file button (

) allows you to write various types of files.The files available for writing include

all those available through the File/Write ribbon tab item, as described in this chapter.

Mesh files are created using the mesh generators (ANSYS Meshing, the meshing mode of Fluent, Fluent

Meshing, GAMBIT, GeoMesh, and PreBFC), or by several third-party CAD packages. From the point of

view of ANSYS Fluent, a mesh file is a subset of a case file (described in Reading and Writing Case

Files (p. )). The mesh file contains the coordinates of all the nodes, connectivity information that tells

how the nodes are connected to one another to form faces and cells, and the zone types and numbers

of all the faces (for example, wall-, pressure-inlet-, symmetry-).

The mesh file does not contain any information on boundary conditions, flow parameters. For information

about meshes, see Reading and Manipulating Meshes (p. ).

To read a native-format mesh file (that is, a mesh file that is saved in the ANSYS Fluent format, which

includes FLUENT /, Fluent/UNS, or RAMPANT meshes) into Fluent, use the File/Read/Mesh... ribbon

tab item.

File → Read → Mesh...

Note that you can also use the File/Read/Case... ribbon tab item (described in Reading and Writing

Case Files (p. )), because a mesh file is a subset of a case file. ANSYS Meshing, the meshing mode of

Fluent, Fluent Meshing, GAMBIT, GeoMesh, and PreBFC can all write a native-format mesh file. For in-

formation about these files and how they are created, see ANSYS Meshing Mesh Files (p. ), Fluent

Meshing Mode Mesh Files (p. ), Fluent Meshing Mesh Files (p. ), GAMBIT Mesh Files (p. ), Geo-

Mesh Mesh Files (p. ), and PreBFC Mesh Files (p. ).

If after reading in a mesh file (or a case and data file), you would like to read in another mesh file, the

Read Mesh Options Dialog Box (p. ) will open, where you can choose to

Discard the case and read in a new mesh.

Replace the existing mesh.

You also have the option to have the Scale Mesh dialog box appear automatically for you to check or

scale your mesh, which in general is the recommended practice. For this to happen, enable Show Scale

Mesh Panel After Replacing Mesh.

For information on importing an unpartitioned mesh file into the parallel version of Fluent using the

partition filter, see Using the Partition Filter (p. ).

For information about reading surface mesh files, see Reading Surface Mesh Files (p. ).

Information related to the ANSYS Fluent simulation is stored in both the case file and the data file. The

commands for reading and writing these files are described in the following sections, along with com-

mands for the automatic saving of case and data at specified intervals.

ANSYS Fluent can read and write either text or binary case and data files. Binary files require less storage

space and are faster to read and write. By default, ANSYS Fluent writes files in binary format. To write

a text file, disable the Write Binary Files check button in the Select File dialog box. In addition, you

can read and write either text or binary files in compressed formats (For details, see Reading and Writing

Compressed Files (p. )). ANSYS Fluent automatically detects the file type when reading.

Furthermore, when writing case and data files, ANSYS Fluent can improve I/O performance using

asynchronous file compression which can be enabled using the Optimize Using Asynchronous I/O

check button in the Select File dialog box.

This option is particularly beneficial if you want to improve the overall performance of simulations in-

volving solution check-pointing. Performance is improved by overlapping the file compression and file

system copy operations with subsequent iterations or other operations. It is best if the front end Cortex

Reading and Writing Case and Data Files

process has its own dedicated processor core (or machine) not used by the ANSYS Fluent compute-

node processes, even though the option would aid performance even if they reside on the same machine.

Important

The Optimize Using Asynchronous I/O option is not available on Windows machines.

If you adapt the mesh, you must save a new case file as well as a data file. Otherwise, the new

data file will not correspond to the case file (for example, they will have different numbers of

cells). If you have not saved the latest case or data file, ANSYS Fluent will warn you when you try

to exit the program.

... Reading and Writing Case Files

... Reading and Writing Data Files

... Reading and Writing Case and Data Files Together

... Reading and Writing Files Using Hierarchical Data Format (HDF)

... Automatic Saving of Case and Data Files

It also contains the information about the user interface and graphics environment. For information

about the format of case files see Case and Data File Formats (p. ). The commands used for reading

case files can also be used to read native-format mesh files (as described in Reading Mesh Files (p. ))

because the mesh information is a subset of the case information. Select the File/Read/Case... ribbon

tab item to open the Select File dialog box.

File → Read → Case...

Read a case file using the Select File dialog box. Note that the Display Mesh After Reading option

in the Select File dialog box allows you to have the mesh displayed automatically after it is read.

Select the File/Write/Case... ribbon tab item to open the Select File dialog box.

File → Write → Case...

Write a case file using the Select File dialog box.

When ANSYS Fluent reads a case file, it first looks for a file with the exact name you typed. If a file with

that name is not found, it searches for the same file with different extensions (Reading and Writing

Compressed Files (p. )). When ANSYS Fluent writes a case file, .cas is added to the name you type

unless the name already ends with .cas.

In the single-precision version of ANSYS Fluent, nodal coordinates are written by default in double

precision, in order to ensure that there is no loss of precision if the case file is read back into the

meshing mode. You can reduce the precision and case file size by using the following text command

prior to writing:

file → single-precision-coordinates?

Data files contain the values of the specified flow field quantities in each mesh element and the con-

vergence history (residuals) for that flow field. For information about the format of data files see Case

and Data File Formats (p. ).

. After reading a mesh or case file, select the File/Read/Data... ribbon tab item to open the Select File

File → Read → Data...

. Read a data file using the Select File dialog box.

. After generating data for a case file, select the File/Write/Data... ribbon tab item to open the Select File

File → Write → Data...

. Write a data file using the Select File dialog box.

When ANSYS Fluent reads a data file, it first looks for a file with the exact name you typed. If a file

with that name is not found, it searches for the same file with different extensions (Reading and

Writing Compressed Files (p. )). When ANSYS Fluent writes a data file, .dat is added to the name

you type unless the name already ends with .dat.

You can output additional quantities for post-processing in other applications using the Data File

Quantities dialog box (see Setting Data File Quantities (p. )).

A case file and a data file together contain all the information required to restart a solution. Case files

contain the mesh, boundary and cell zone conditions, and solution parameters. Data files contain the

values of the flow field in each mesh element and the convergence history (residuals) for that flow

field.

field.

You can read a case file and a data file together by using the Select File dialog box opened by selecting

the File/Read/Case & Data... ribbon tab item. To read both files, select the appropriate case file, and

the corresponding data file (same name with .dat suffix) is also read. Note that the Display Mesh

After Reading option in the Select File dialog box allows you to have the mesh displayed automatically

after it is read.

File → Read → Case & Data...

To write a case file and a data file, select the File/Write/Case & Data... ribbon tab item.

File → Write → Case & Data...

When reading and writing case and data files in serial or parallel, you can optionally use the Hierarch-

ical Data Format (HDF). To read or write case/data files using HDF, you can use the same GUI or TUI

commands as you normally would and simply append .h5 to the file name. Alternatively, you can

select HDF5 Case Files or HDF5 Data Files from the Files of type drop-down list in the Select File

dialog box. If you want to write HDF files automatically at specified intervals during a calculation, do

not append .h5 to the file name in the Autosave Dialog Box (p. ), but instead set HDF as the default

for reading and writing files by using the following text command:

file → hdf-files?

Note

HDF files are not supported in Fluent Meshing or when running Fluent under ANSYS

Workbench.

Note

text editor. However, third-party tools are available that allow you to open and explore the contents

You can specify the I/O mode and/or the HDF compression level through text commands:

> file hdfio-options compression-level

compression-level [-]? []

>  file hdfio-options io-mode

HDF5 I/O Modes:

. HOST

. NODE0

. PARALLEL INDEPENDENT

. PARALLEL COLLECTIVE

Enter Mode Number: []

HOST mode selected.

The compression level can be set from  (no compression; fastest) to  (maximum compression;

slowest); the default level is . Note that increasing the compression level may not necessarily yield a

corresponding decrease in file size.

The available I/O modes are:

HOST: I/O is done serially by the host process. This is the default mode when the file path is

not accessible to compute-node .

NODE0: I/O is done serially by the node  process. This is the default mode when the file path

is accessible to compute-node .

PARALLEL INDEPENDENT: I/O is done in a parallel file system using the independent mode

of MPI I/O.

PARALLEL COLLECTIVE: I/O is done in a parallel file system using the collective mode of MPI

I/O.

Note

The Parallel I/O modes do not support compression. If you have specified a non-zero level for

compression and you switch to one of the parallel modes, the compression will be set to .

When using the double-precision solver, you can specify that the data written in HDF data files is single

precision (and thus sacrifice some precision in order to reduce the size of the files) by using the following

text command prior to writing:

file → hdfio-options → single-precision-data?

You can request ANSYS Fluent to automatically save case and data files at specified intervals during a

calculation. This is especially useful for time-dependent calculations, since it allows you to save the

results at different time steps, flow times, or crank angles (for in-cylinder simulations) without stopping

the calculation and performing the save manually. You can also use the autosave feature for steady-

state problems, and thus examine the solution at different stages in the iteration history.

Automatic saving is specified using the Autosave Dialog Box (p. ) (Figure . : The Autosave Dialog

Box (p. )), which is opened by clicking the Edit... button next to the Autosave Every text box in

the Calculation Activities task page.

Calculation Activities

Figure . : The Autosave Dialog Box

Specify how often you would like to save your modified files by entering the frequency in the Save

Data File Every number-entry field. Save Data File Every is set to zero by default, indicating that no

automatic saving is performed.

For transient in-cylinder simulations, specify whether you want to save the data by Time Steps or

Crank Angles.

If you choose to save the case file only if it is modified, then select Only if modified under Save As-

sociated Case Files. Note that the case file will be saved whether you make a manual change, or if

ANSYS Fluent makes a change internally during the calculation. If you choose to save the case file

every time the data file is saved, then select Each Time.

Important

To save only the data files, use the following TUI option:

file → auto-save → case-frequency → if-mesh-is-modified

This will result in the options in the Save Associated Case Files group box being disabled

in the Autosave dialog box. In essence, this TUI command forces ANSYS Fluent to the save

case file only when the mesh is modified. It does not disable case file saving, but reduces

it to an absolute minimum. This is necessary to do so since you cannot read a data file

without a case file containing a matching mesh.

For steady-state solutions, specify the frequency in iterations. For transient solutions, specify it in time

steps (unless you are using the explicit time stepping formulation, in which case specify the frequency

in iterations). For transient in-cylinder solutions, you can choose to specify the frequency in crank

angles. If you define a frequency of , for example, a case file is saved every  iterations, time steps,

or crank angles.

If you have limited disk space, restrict the number of files saved by ANSYS Fluent by selecting the Retain

Only the Most Recent Files option. When selected, enter the Maximum Number of Data Files you

would like to retain. Note that the case and data files are treated separately with regard to the maximum

number of files saved when overwriting. For example, if the value of Maximum Number of Data Files

is set to five, ANSYS Fluent saves a maximum of five case and five data files, irrespective of the frequency.

After the maximum limit of files has been saved, ANSYS Fluent begins overwriting the earliest existing

file.

Note

When the Retain only the Most Recent Files option is selected, the solution history currently

in memory will be discarded and the solution history reset.

If you have generated data (either by initializing the solution or running the calculation) you can view

the list of standard quantities that will be written to the data file as a result of the autosave, and even

select additional quantities for postprocessing in alternative applications. Click the Data File Quantities...

button to open the Data File Quantities dialog box, and make any necessary selections. For details,

see Setting Data File Quantities (p. ).

Enter a root name for the autosave files in the File Name text box. When the files are saved, a number

will be appended to this root name to indicate the point at which it was saved during the calculation:

for steady-state solutions, this will be the iteration number, whereas for transient solutions it will be

either the time step number, flow time, or crank angle (depending on your selection in the step that

follows). An extension will also be automatically added to the root name (.cas or .dat). If the specified

File Name ends in .gz or .Z, appropriate file compression is performed. For details about file com-

pression, see Reading and Writing Compressed Files (p. ). For details on autosaving files in the

hierarchical data format (HDF), see Reading and Writing Files Using Hierarchical Data Format

(HDF) (p. ).

For transient calculations, make a selection from the Append File Name with drop-down list to indicate

whether you want the root file name to be appended with the time-step, flow-time or crank-angle

(see Figure . : The Autosave Dialog Box (p. )). If you select either of the latter two, you can set the

Decimal Places in File Name to determine the ultimate width of the file name.

Consider a transient case for which you want to save your case and data files at known time steps.

The procedure you would follow is to first set the frequency in the Save Data File Every text box.

Select Each Time if you want both case and data files saved at the same interval. Then enter my_file

for the File Name. Finally, select time-step from the Append File Name with drop-down list. An ex-

ample of the resulting files saved would be

my_file-.cas

my_file-.dat

indicating that these files were saved at the fifth time step.

You can revise the instructions for the previous example to instead save case and data files at known

flow times, by selecting flow-time from the Append File Name with drop-down list. The default

Decimal Places in File Name will be six. An example of the resulting files saved would be

my_file-..cas

my_file-..dat

indicating that these files were saved at a flow time of . seconds.

For steady-state and transient cases, you have the option of automatically numbering the files (as de-

scribed in Automatic Numbering of Files (p. )), and thereby include further information about when

the files were saved. This involves the addition of special characters to the File Name. For example,

you may want the file names to convey the flow times with their corresponding time steps (transient

cases only). Select time-step from the Append File Name with, and enter a File Name that ends with

%f to automatically number the files with the flow time. Thus, entering a File Name of filename-

%f could result in a saved case file named filename-.-.cas. The conventions

used in this example can be explained as follows:

filename- is the file name you entered when autosaving your solution.

. is the result of the special character %f added to the file name, and is the flow time.This

flow time has a field width of ten characters, which allows for six decimal places (as discussed in Automatic

Numbering of Files (p. )).

- is the appended time-step, as designated by the selection in the Append File Name with drop-

down list.

.cas is the file extension automatically added when using the autosave option.

All of the autosave inputs are stored in memory when you click OK in the Autosave dialog box, and

can then be saved with the case file.

Case files created by Fluent/UNS  or  or RAMPANT , , or  can be read into ANSYS Fluent in the

same way that current case files are read (see Reading and Writing Case and Data Files (p. )). If you

read a case file created by Fluent/UNS, ANSYS Fluent selects Pressure-Based in the Solver group box

of the General Task Page (p. ). If you read a case file created by RAMPANT, ANSYS Fluent selects

Reading Fluent/UNS and RAMPANT Case and Data Files

Density-Based in the Solver group box of the General Task Page (p. ), as well as Explicit from the

Formulation drop-down menu in the Solution Methods Task Page (p. ).

Data files created by Fluent/UNS  or RAMPANT  can be read into ANSYS Fluent in the same way that

current data files are read (see Reading and Writing Case and Data Files (p. )).

Boundary profiles are used to specify flow conditions on a boundary zone of the solution domain. For

example, they can be used to prescribe a velocity field on an inlet plane. For information on boundary

profiles, see Profiles (p. ). For information about transient profiles, see Defining Transient Cell Zone

and Boundary Conditions (p. ).

... Reading Profile Files

...Writing Profile Files

To read the boundary profile files, open the Select File dialog box by selecting the File/Read/Profile...

ribbon tab item.

File → Read → Profile...

This opens the Select File dialog box so that you can read a boundary profile with the standard exten-

sion .prof or a transient profile in tabular format with the standard extension .ttab. If a profile in

the file has the same name as an existing profile, the old profile will be overwritten.

Note

The maximum number of profiles that can be read into a single Fluent session is .

You can also create a profile file from the conditions on a specified boundary or surface. For example,

you can create a profile file from the outlet conditions of one case. Then you can read that profile into

another case and use the outlet profile data as the inlet conditions for the new case.

To write a profile file, use the Write Profile Dialog Box (p. ) (Figure . : The Write Profile Dialog

Box (p. )).

File → Write → Profile...

Figure . : The Write Profile Dialog Box

. Retain the default option of Define New Profiles.

. Select the surface(s) from which you want to extract data for the profile(s) in the Surfaces list.

. Choose the variable(s) for which you want to create profiles in the Values list.

. Optionally select Write Merge Profiles.This writes a .csv file with the selected surfaces consolidated

into one set of data points. Note that this option is only available if you have selected  or more surfaces.

. Click Write... and specify the profile file name in the resulting Select File dialog box.

ANSYS Fluent saves the mesh coordinates of the data points for the selected surface(s) and the

values of the selected variables at those positions. When you read the profile file back into Fluent,

you can select the profile values from the relevant drop-down lists in the boundary condition dialog

boxes. The names of the profile values in the drop-down lists will consist of the surface name and

the particular variable.

. Select the Write Currently Defined Profiles option:

if you have made any modifications to the boundary profiles since you read them in (for example, if

you reoriented an existing profile to create a new one).

if you want to store all the profiles used in a case file in a separate file.

Reading and Writing Profile Files

. Click Write... and specify the file name in the resulting Select File dialog box. All currently defined profiles

are saved in this file.This file can be read back into Fluent whenever you want to use these profiles again.

To save all currently defined boundary conditions to a file, enter the file/write-settings text

command and specify a name for the file.

file → write-settings

ANSYS Fluent writes the boundary and cell zone conditions, the solver, and model settings to a file using

the same format as the “zone” section of the case file. See Case and Data File Formats (p. ) for details

about the case file format.

To read boundary conditions from a file and to apply them to the corresponding zones in your model,

enter the file/read-settings text command.

file → read-settings

ANSYS Fluent sets the boundary and cell zone conditions in the current model by comparing the zone

name associated with each set of conditions in the file with the zone names in the model. If the model

does not contain a matching zone name for a set of boundary conditions, those conditions are ignored.

If you read boundary conditions into a model that contains a different mesh topology (for example, a

cell zone has been removed), check the conditions at boundaries within and adjacent to the region of

the topological change. This is important for wall zones.

Note

If the boundary conditions are not checked and some remain uninitialized, the case will not

run successfully.

When the file/read-settings text command is not used, all boundary conditions get the default

settings when a mesh file is imported, allowing the case to run with the default values.

If you want ANSYS Fluent to apply a set of conditions to multiple zones with similar names, or to a

single zone with a name you are not sure of in advance, you can edit the boundary-condition file saved

with the file/write-settings command to include wildcards (*) within the zone names. For ex-

ample, if you want to apply a particular set of conditions to wall-, wall-, and wall- in your current

model, edit the boundary-condition file so that the zone name associated with the desired conditions

is wall-*.

Note

The settings file contains only your user-modified settings and does not include default

ANSYS Fluent parameters. The default parameters may be updated with each new release.

Consequently, the usage of the same settings file in different releases of ANSYS Fluent

does not guarantee the same setup, which can cause solution differences.

You can write the boundary zones (surface mesh) to a file. This file can be read and used by the

meshing mode of Fluent to produce a volume mesh. You may find this feature useful if you are unsat-

isfied with a mesh obtained from another mesh generation program.

A boundary mesh can be written using the Select File dialog box, opened by selecting the

File/Write/Boundary Mesh... ribbon tab item.

File → Write → Boundary Mesh...

For large source files, use the Select File dialog box, opened by selecting the File/Read/Scheme...

ribbon tab item

File → Read → Scheme...

or use the Scheme load function in the console, as shown in the following example:

Shorter files can also be loaded with the File/Read/Journal... ribbon tab item or the file/ read-

journal command in the text interface (or its . or source alias, as shown in the example that follows).

>. file.scm

In this case, each character of the file is echoed to the console as it is read, in the same way as if you

were typing in the contents of the file.

A journal file contains a sequence of ANSYS Fluent commands, arranged as they would be typed inter-

actively into the program or entered through the GUI or TUI. The GUI and TUI commands are recorded

as Scheme code lines in journal files. You can also create journal files manually with a text editor. If you

want to include comments in your file, be sure to put a semicolon (;) at the beginning of each comment

line. See Background Execution on Linux Systems (p. ) in the Getting Started Guide for an example.

on the command line. Another use is to produce a record of the input to a program session for later

reference, although transcript files are often more useful for this purpose. (For details, see Creating

Transcript Files (p. )).

Important

A journal file is, by design, just a simple record and playback facility. It contains no information

about the state in which it was recorded (other than the version of ANSYS Fluent that it was

created in) or the state in which it is being played back.

The precision (single or double) that the journal is recorded in may affect playback when it is

read into a session that is running in the other precision.

Be careful not to change the folder while recording a journal file. Also, try to re-create the state in which the

journal was written before you read it into the program. For example, if your journal file includes an instruction

to save a new file with a specified name, you should check that if a file with that name exists in your folder

before you read in your journal file. If a file with that name exists and you read in your journal file, when the

program reaches the write instruction, it will prompt for a confirmation to overwrite the old file.

Since the journal file does not contain any response to the confirmation request, ANSYS Fluent cannot

continue to follow the instructions of the journal file.

Other conditions that may affect the program’s ability to perform the instructions contained in a journal file

For example, if your journal file creates several surfaces and displays data on those surfaces, you must

be sure to read in appropriate case and data files before reading the journal file.

Important

At a point of time, only one journal file can be open for recording, but you can write a

journal and a transcript file simultaneously. You can also read a journal file at any time.

Note

journal.

Whether you choose to type the text command in full or use partial strings (as described in Command

Abbreviation), complete commands are recorded in the journal files. Consider the following examples:

Typing in the TUI

solve/set/expert , , yes , ,

will be recorded in the journal file as

/solve/set/expert yes no yes no no

where , or Enter signifies default values or entries, as described in Text Prompt System.

so set ur mom . pres .

will be recorded in the journal file as two separate commands:

/solve/set/under-relaxation/mom .

/solve/set/under-relaxation/pressure .

Important

Only successfully completed commands are recorded. For example, if you stopped an execution

of a command using Ctrl+c, it will not be recorded in the journal file.

If a GUI event happens while a text command is in progress, the GUI event is recorded first.

All default values are recorded (as in the first example above).

For additional information, see the following section:

... Procedure

... Multiple Journal Files

To start the journaling process, select the File/Write/Start Journal... ribbon tab item.

File → Write → Start Journal...

After you enter a name for the file in the Select File dialog box, journal recording begins. The Start

Journal... menu item becomes the Stop Journal menu item. You can end journal recording by selecting

Stop Journal, or by exiting the program.

File → Write → Stop Journal

You can read a journal file into the program using the Select File dialog box opened by selecting the

File/Read/Journal... ribbon tab item.

File → Read → Journal...

Journal files are always loaded in the main (that is, top-level) text menu, regardless of where you are

in the text menu hierarchy when you invoke the read command.

It is possible to read multiple journal files into Fluent at once.

To read multiple journal files through the Select File dialog box:

. Open the Select File dialog box.

. Select your files in the order you want them read into Fluent.

The order in which they will be read is indicated by the red box in Figure . : Multiple Selection of

Journal Files (p. ).

Figure . : Multiple Selection of Journal Files

. Click OK to load the selected files.

Nested Journal Files

It is possible to create a journal file that makes calls to other journal files.

The following is an example of a nested journal file:

A transcript file contains a complete record of all standard input to and output from ANSYS Fluent (usually

all keyboard and GUI input and all screen output). GUI commands are recorded as Scheme code lines

in transcript files. ANSYS Fluent creates a transcript file by recording everything typed as input or entered

through the GUI, and everything printed as output in the text window.

The purpose of a transcript file is to produce a record of the program session for later reference. Because

they contain messages and other output, transcript files (unlike journal files), cannot be read back into

the program.

Important

Only one transcript file can be open for recording at a time, but you can write a transcript

To start the transcription process, select the File/Write/Start Transcript... ribbon tab item.

File → Write → Start Transcript...

After you enter a name for the file in the Select File dialog box, transcript recording begins and the

Start Transcript... menu item becomes the Stop Transcript menu item.

You can end transcript recording by selecting Stop Transcript, or by exiting the program.

File → Write → Stop Transcript

ANSYS Fluent allows you to import the following file formats:

ABAQUS  .inp, .fil, and .odb files*

CFX  .def and .res files

CGNS files*

EnSight files*

ANSYS FIDAP files*

GAMBIT files

HYPERMESH ASCII files*

I-deas Universal files*

LSTC/DYNA keyword input files and state databases*

Marc POST files*

Mechanical APDL  .inp, .cdb, .rst, and .rmg files*

NASTRAN Bulk Data files*

PATRAN Neutral files*

PLOT3D mesh files*

PTC Mechanica Design studies*

Tecplot files*

Requires a VKI license

Figure . : The Import Menu

Important

Once you have imported any 3rd party file it is recommended that you confirm that the

boundary zones and cell zones are set up as you expect.

For information on importing particle history data, see Importing Particle Data (p. ).

... ABAQUS Files

... CFX Files

... Meshes and Data in CGNS Format

... EnSight Files

... ANSYS FIDAP Neutral Files

... GAMBIT and GeoMesh Mesh Files

... HYPERMESH ASCII Files

... I-deas Universal Files

... LSTC Files

... Marc POST Files

... Mechanical APDL Files

... NASTRAN Files

... PATRAN Neutral Files

... PLOT3D Files

... PTC Mechanica Design Files

...Tecplot Files

... Fluent  Case Files

... PreBFC Files

... Partition Files

... CHEMKIN Mechanism

To import an ABAQUS input file, use the File/Import/ABAQUS/Input File... ribbon tab item.

File → Import → ABAQUS → Input File...

Select this menu item to open the Select File dialog box. Specify the name of the ABAQUS Input File

to be read. The ABAQUS input file (.inp) is a text file that contains the input description of a finite

element model for the ABAQUS finite element program. The interface only produces datasets associated

with the finite element model, no results of datasets are produced. Element types commonly associated

with structural analysis are supported by this file format. There is a list of input keywords that are re-

cognized in the ABAQUS Input File [] (p. ).

To import an ABAQUS filbin file, use the File/Import/ABAQUS/Filbin File... ribbon tab item.

File → Import → ABAQUS → Filbin File...

Select this menu item to open the Select File dialog box. Specify the name of the ABAQUS Filbin File

to be read. This output file has a .fil extension and consists of finite element model and results

data.

To import an ABAQUS ODB file, use the File/Import/ABAQUS/ODB File... ribbon tab item.

File → Import → ABAQUS → ODB File...

Select this menu item to open the Select File dialog box. Specify the name of the ABAQUS ODB File

to be read. This output database file has a .odb extension and consists of finite element model and

results data in the OpenDocument format.

To import a CFX definition file, use the File/Import/CFX/Definition File... ribbon tab item.

File → Import → CFX → Definition File...

Select this menu item to open the Select File dialog box. Specify the name of the CFX Definition File

to be read. Fluent reads mesh information from the CFX file with .def extensions. For information

about importing CFX files, see CFX Files (p. ).

To import a CFX result file, use the File/Import/CFX/Result File... ribbon tab item.

File → Import → CFX → Result File...

In the Select File dialog box, specify the name of the CFX Result File to be read. Those imported files

will have .res extensions.

Note that the Create Zones from CCL Physics Data option in the Select File dialog boxes allows you

to create zones from the physics data objects or the primitive mesh region objects.

Important

CFX file import is available for 3D cases only.

To import meshes in CFD general notation system (CGNS) format (.cgns) into ANSYS Fluent, use the

File/Import/CGNS/Mesh... ribbon tab item.

File → Import → CGNS → Mesh...

To import a mesh and the corresponding CGNS data, use the File/Import/CGNS/Mesh & Data... ribbon

tab item.

File → Import → CGNS → Mesh & Data...

To import only the CGNS data, use the File/Import/CGNS/Data... ribbon tab item.

File → Import → CGNS → Data...

Table . : CGNS Variables Supported by ANSYS Fluent

ANSYS Fluent Name

CGNS Variable Name

pressure

Pressure

uu-stress

ReynoldsStressXX

uv-stress

ReynoldsStressXY

uw-stress

ReynoldsStressXZ

vv-stress

ReynoldsStressYY

vw-stress

ReynoldsStressYZ

pressure

Pressure

uu-stress

uv-stress

uw-stress

vv-stress

vw-stress

ww-stress

ReynoldsStressZZ

temperature

Temperature

epsilon

TurbulentDissipation

omega

TurbulentDissipationRate

k

TurbulentEnergyKinetic

x-velocity

VelocityX

y-velocity

VelocityY

z-velocity

VelocityZ

Important

To import data correctly, first import the mesh using the mesh only option (Mesh...) and set up

the boundary conditions. For example, if a boundary zone is of type pressure-outlet and is read

as outlet, it should be changed to pressure-outlet before importing the data.Then select the

appropriate model and read the data using the data only option (Data...)

The new and original meshes should have the same zones, numbered in the same order. A

warning is issued if they do not, because inconsistencies can create problems with the boundary

conditions.

ANSYS Fluent defaults to the Laminar Viscous Model after reading a CGNS mesh.You must

select the appropriate model before reading data since ANSYS Fluent selectively imports only

those values from the CGNS file required for a given model. For example, if Epsilon is available

in the CGNS file, the model must be changed to k-epsilon to ensure that ANSYS Fluent will

import this quantity.

You can import an EnSight file using the File/Import/EnSight... ribbon tab item.

File → Import → EnSight...

This file format is applied to both unstructured and structured data, where each part contains its own

local coordinate array. The EnSight Gold software package, which uses this file format, allows you to

analyze, visualize, and communicate engineering datasets. It allows you to take full advantage of par-

allel processing and rendering and supports a range of virtual reality devices. Furthermore, it enables

real-time collaboration.

When selecting this option, the Select File dialog box will appear, where you will specify a file name.

This file will have an .encas or .case extension.

Only the mesh file is read into ANSYS Fluent, and any data present is discarded.

You can read an ANSYS FIDAP neutral file using the File/Import/FIDAP... ribbon tab item.

File → Import → FIDAP...

In the Select File dialog box, specify the name of the ANSYS FIDAP Neutral File to be read. This file

will have an .FDNEUT or .unv file extension. ANSYS Fluent reads mesh information and zone types

from the ANSYS FIDAP file. You must specify boundary conditions and other information after reading

this file. For information about importing ANSYS FIDAP Neutral files, see ANSYS FIDAP Neutral

Files (p. ).

If you have saved a neutral file from GAMBIT, rather than an ANSYS Fluent mesh file, you can import

it into ANSYS Fluent using the File/Import/GAMBIT... ribbon tab item.

File → Import → GAMBIT...

For information about importing files from GAMBIT and GeoMesh, see GAMBIT Mesh Files (p. ) and

GeoMesh Mesh Files (p. ).

You can read a HYPERMESH ASCII file using the File/Import/HYPERMESH ASCII... ribbon tab item.

File → Import → HYPERMESH ASCII...

HYPERMESH is a high-performance finite element pre- and postprocessor for popular finite element

solvers, allowing engineers to analyze product design performance in a highly interactive and visual

This file should have an .hm, .hma, or .hmascii extension.

I-deas Universal files can be read into ANSYS Fluent with the File/Import/I-deas Universal... ribbon

tab item.

File → Import → I-deas Universal...

Select the I-deas Universal... menu item to open the Select File dialog box.

Specify the name of the I-deas Universal file to be read. Fluent reads mesh information and zone types

from the I-deas Universal file. For information about importing I-deas Universal files, see I-deas Univer-

sal Files (p. ).

To import an LSTC input file, use the File/Import/LSTC/Input File... ribbon tab item.

File → Import → LSTC → Input File...

The LSTC input file is a text file that contains the input description of a finite element model for the

LS-DYNA finite element program. This interface only produces datasets associated with the mesh, no

results datasets are produced. The element types commonly associated with structural analysis are

supported.

LSTC input files have the following file extensions: .k, .key, and .dyn

To import an LSTC state file, use the File/Import/LSTC/State File... ribbon tab item.

File → Import → LSTC → State File...

The state file consists of three major sections: control data, geometry data, and state data. Each dataset

in the state data section corresponds to the time and global data items associated with each state on

the database. Dataset attributes include such things as time, energy, and momentum.

An LSTC state file has a .d3plot file extension.

Marc POST files can be read into ANSYS Fluent using the File/Import/Marc POST... ribbon tab item.

File → Import → Marc POST...

Select the Marc POST... menu item and in the Select File dialog box, specify the name of the file to

be read.

These files are generated using MSC Marc, a nonlinear finite element program. MSC Marc allows you

to study deformations that exceed the linear elastic range of some materials, enabling you to assess

the structural integrity and performance of the material. It also allows you to simulate deformations

that are part-to-part or part-to-self contact under a range of conditions.

To import a Mechanical APDL input file, use the File/Import/Mechanical APDL/Input File... ribbon

tab item.

File → Import → Mechanical APDL → Input File...

Select this menu item to open the Select File dialog box. Specify the name of the Mechanical AP-

DL Prep7 File to be read. Fluent reads mesh information from the Mechanical APDL file with .ans,

.neu, .cdb, and .prep7 extensions. For information about importing Mechanical APDL files, see

Mechanical APDL Files (p. ).

To import a Mechanical APDL result file, use the File/Import/Mechanical APDL/Result File... ribbon

tab item.

File → Import → Mechanical APDL → Result File...

In the Select File dialog box. Specify the name of the Mechanical APDL Result File to be read. Those

imported files will have .rst, .rth, and .rmg extensions.

You can read NASTRAN Bulkdata files into ANSYS Fluent with the File/Import/NASTRAN/Bulkdata

File... ribbon tab item.

File → Import → NASTRAN → Bulkdata File...

When you select the Bulkdata File... menu item, the Select File dialog box will appear and you will

specify the name of the NASTRAN File to be read. This file will have .nas, .dat, .bdf file extensions.

Fluent reads mesh information from the NASTRAN file. For information about importing NASTRAN files,

see NASTRAN Files (p. ).

To import NASTRAN Op2 files into ANSYS Fluent, use the File/Import/NASTRAN/Op2 File... ribbon

tab item.

File → Import → NASTRAN → Op2 File...

In the Select File dialog box, specify the name of the NASTRAN Output2 File to be read. This file is

an output binary data file that contains data used in the NASTRAN finite element program. This file

will have .op2 file extension.

To read a PATRAN Neutral file zoned by named components (that is, a file in which you have grouped

nodes with the same specified group name), use the File/Import/PATRAN Neutral... ribbon tab item.

File → Import → PATRAN Neutral...

Selecting this menu item opens the Select File dialog box. Specify the name of the PATRAN Neutral file

to be read (extension .neu, .out, or .pat). Fluent reads mesh information from the PATRAN Neut-

ral file. For information about importing PATRAN Neutral files, see PATRAN Neutral Files (p. ).

To import a PLOT3D mesh file, use the File/Import/PLOT3D Grid... ribbon tab item.

File → Import → PLOT3D Grid...

The PLOT3D mesh files have .p3d, .bin, .x, .xyz, or .grd file extensions.

These file formats may be formatted, unformatted or binary.

To import a PTC Mechanica Design file, use the File/Import/PTC Mechanica Design... ribbon tab item.

File → Import → PTC Mechanica Design...

This will open the Select File dialog box. Specify the name of the neutral file to be read.

The PTC Mechanica Design file contains analysis, model and results data. Only the binary form of the

results data files is supported.

The form of the file must have the .neu extension.

Important

Mechanica results consists of an entire directory structure of files, called a “study” in Mech-

anica terminology, which must be used in exactly the form that Mechanica originally gen-

erates it. ANSYS Fluent’s VKI interface keys on the .neu file and can traverse the directory

structure from there to access the other files that it needs.

To import a Tecplot file, use the File/Import/Tecplot... ribbon tab item.

File → Import → Tecplot...

The Tecplot file is a binary file. Only the mesh is read into ANSYS Fluent and any data present is dis-

carded.

The form of the file must have the .plt extension. ANSYS Fluent supports the importation of poly-

hedral cells and files created by Tecplot version .–., except for version . (which is unsupported).

You can read a Fluent  case file using the File/Import/Fluent  Case File... ribbon tab item.

File → Import → Fluent  Case File...

Select the Fluent  Case File... menu item to open the Select File dialog box. Specify the name of

the Fluent  case file to be read. ANSYS Fluent reads only mesh information and zone types from the

Fluent  case file. You must specify boundary and cell zone conditions, model parameters, material

properties, and other information after reading this file. For information about importing Fluent  case

files, see FLUENT  Case Files (p. ).

You can read a PreBFC structured mesh file into ANSYS Fluent using the File/Import/PreBFC File...

File → Import → PreBFC File...

Select the PreBFC File... menu item to open the Select File dialog box. Specify the name of the

PreBFC structured mesh file to be read. Fluent reads mesh information and zone types from the PreB-

FC mesh file. For information about importing PreBFC mesh files, see PreBFC Mesh Files (p. ).

To perform METIS partitioning on an unpartitioned mesh, use the File/Import/Partition/Metis... ribbon

tab item.

File → Import → Partition → Metis...

You may also partition each cell zone individually, using the File/Import/Partition/Metis Zone... ribbon

tab item.

File → Import → Partition → Metis Zone...

See Using the Partition Filter (p. ) for detailed information about partitioning.

To import a CHEMKIN format, you can import the mechanism file into ANSYS Fluent using the

File/Import/CHEMKIN Mechanism... ribbon tab item (Figure . : The Import CHEMKIN Format

Mechanism Dialog Box for Volumetric Kinetics (p. )).

File → Import → CHEMKIN Mechanism...

See Importing a Volumetric Kinetic Mechanism in CHEMKIN Format (p. ) for detailed information on

importing a CHEMKIN Mechanism file.

The current release of ANSYS Fluent allows you to export data to ABAQUS, , Mechanical APDL Input,

ASCII, AVS, CDAT for CFD-Post and EnSight, CGNS, Data Explorer, EnSight, FAST, FIELDVIEW, I-deas,

NASTRAN, PATRAN, TAITherm, and Tecplot formats. Exporting Solution Data after a Calculation (p. )

explains how to export solution data in these formats after the calculation is complete, and ABAQUS

Files (p. ) to Tecplot Files (p. ) provide specific information for each type of File Type. For inform-

ation about exporting solution data during transient flow solutions, see Exporting Data During a Tran-

sient Calculation (p. ).

For NASTRAN, ABAQUS, Mechanical APDL Input, I-deas Universal, and PATRAN file formats, the following

quantities are exported [] (p. ):

Nodes, Elements

Node Sets (Boundary Conditions)

Pressure

Heat Flux

Heat Transfer Coefficient

Force

To generate the force data that is exported for nodes at boundaries, ANSYS Fluent performs the fol-

lowing steps:

. Facial force for each wall face is calculated by summing the pressure force, viscous force and surface

tension force of the face.

Exporting Solution Data

. Partial force for each wall face is calculated by dividing its facial force by its number of shared nodes.

. Total force for each wall node is calculated by summing the partial forces of all the wall faces sharing

that node.

that node.

... Exporting Limitations

Note the following limitations when exporting solution data:

When using the parallel version of ANSYS Fluent, you can only export to the following packages:

– ABAQUS

– CDAT for CFD-Post and EnSight

– ASCII

– CGNS

– EnSight Case Gold

– Fieldview Unstructured

– I-deas Universal

– Mechanical APDL Input

– NASTRAN

– PATRAN

– TAITherm

Note that parallel TAITherm export is only available for surface data.

– Tecplot

The exported file will be written by the host process (see Introduction to Parallel Processing (p. )).

Note that the memory required to write the file may exceed the memory available to the host process.

When using the serial version of ANSYS Fluent, you can only export surface data for TAITherm software.

The solution mode of Fluent cannot import surfaces. Consequently, if you export a file from ANSYS Fluent

with surfaces selected, you may not be able to read these files back into the solution mode. However, the

meshing mode of Fluent can import surface data (see the Fluent Meshing section of the User’s Guide for

details).

The following file types require a VKI license: ABAQUS, CGNS, Ideas-Universal, NASTRAN, PATRAN,Tecplot

ANSYS Fluent supports exporting polyhedral data only for ASCII, CDAT for CFD-Post and EnSight, CGNS,

EnSight Case Gold, NASTRAN,TAITherm,Tecplot and Fieldview Unstructured file formats. For further details,

see ASCII Files (p. ), CDAT for CFD-Post and EnSight (p. ), CGNS Files (p. ), EnSight Case

Gold Files (p. ), NASTRAN Files (p. ), TAITherm Files (p. ) and FieldView Unstructured Files (p. ).

If the files that are exported during multiple transient simulations are to be used as a set, you must make

sure that all of the simulations are run on the same platform, using the same number of processors.This

ensures that all of the files are compatible with each other.

Data on user defined/created surfaces is not available for export to EnSight Case Gold file format.

To export solution data to a different file format after a calculation is complete, use the Export Dialog

Box (p. ) (Figure . : The Export Dialog Box (p. )).

File → Export → Solution Data...

Figure . : The Export Dialog Box

Information concerning the necessary steps and available options for each File Type are listed in ABAQUS

Files (p. ) to Tecplot Files (p. ).

For details about general limitations for exporting solution data and the manner in which it is exported,

see Exporting Solution Data (p. ).

... Mechanical APDL Input Files

... ASCII Files

... AVS Files

... CDAT for CFD-Post and EnSight

... CGNS Files

... Data Explorer Files

... EnSight Case Gold Files

... FAST Files

Exporting Solution Data after a Calculation

... FAST Solution Files

... FieldView Unstructured Files

... PATRAN Files

...TAITherm Files

Select ABAQUS from the File Type drop-down list and choose the surface(s) for which you want to

write data in the Surfaces list. If no surfaces are selected, the entire domain is exported.

When the Energy Equation is enabled in the Energy Dialog Box (p. ), you can choose the loads to

be written based on the kind of finite element analysis you intend to undertake. By selecting Structural

in the Analysis list, you can select the following Structural Loads: Force, Pressure, and Temperature.

By selecting Thermal in the Analysis list, you can select the following Thermal Loads: Temperature,

Heat Flux, and Heat Trans Coeff. Note the following limitations with these loads:

When the Energy Equation is disabled, only the Structural Loads options of Force and Pressure are

Loads are written only on boundary walls when the entire domain is exported (that is, if no Surfaces are

selected).

Click the Write... button to save the file, using the Select File dialog box. The exported file format of

ABAQUS (file.inp) contains coordinates, connectivity, zone groups, and optional loads.

Export of data to ABAQUS is valid only for solid zones or for those surfaces that lie at the intersection

of solid zones. Temperature data is exported for the whole domain.

You have the option of exporting data at specified intervals during a transient calculation through the

Automatic Export dialog box. See Exporting Data During a Transient Calculation (p. ) for the complete

details.

details.

Select Mechanical APDL Input from the File Type drop-down list and choose the surface(s) for which

you want to write data in the Surfaces list. If no surfaces are selected, the entire domain is exported.

Click the Write... button to save the file, using the Select File dialog box. ANSYS Fluent exports an

input file that contains Mechanical APDL finite element information including nodes, elements, and

loads that can be used to do finite element analysis in Mechanical APDL with minimal effort. The file

format is written in .cdb format. The export of Mechanical APDL Input files is in ASCII format and

therefore is available on all platforms.

details.

details.

Select ASCII from the File Type drop-down list and choose the surface(s) for which you want to write

data in the Surfaces list. If no surfaces are selected, the entire domain is exported. Also select the

variable(s) for which data is to be saved in the Quantities list.

When exporting ASCII files, you have the following options:

Select the Location from which the values of scalar functions are to be taken. If you specify the data Location

as Node, then the data values at the node points are exported. If you choose Cell Center, then the data

values from the cell centers are exported. For boundary faces, it is the face center values that are exported

when the Cell Center option is selected.

Select the Delimiter separating the fields (Comma or Space).

Click the Write... button to save the file, using the Select File dialog box. ANSYS Fluent will export a

single ASCII file containing coordinates, optional loads, and specified scalar function data.

Important

ANSYS Fluent supports exporting polyhedral data to ASCII.

details.

Select AVS from the File Type drop-down list and specify the scalars you want in the Quantities list.

Click the Write... button to save the file, using the Select File dialog box. An AVS version  UCD file

contains coordinate and connectivity information and specified scalar function data.

details.

The default output file for ANSYS Fluent is a .dat file (see Reading and Writing Data Files (p. )),

however, when reading Fluent output into CFD-Post, a .cdat file is strongly preferred. .cdat files

are also compatible with EnSight, although EnSight Case Gold files (EnSight Case Gold Files (p. ))

are recommended for the best performance in EnSight.

Important

When reading .dat files into ANSYS CFD-Post, some variables may show incorrect values

in some conditions. You should use .cdat files instead of .dat files. If you don't, then

you may need to cross check these values between CFD-Post and Fluent.

To export data to files that are compatible with ANSYS CFD-Post and Ensight, select CDAT for CFD-

Post and EnSight from the File Type drop-down list. Next, specify the Cell Zones that contain the

data you want exported; note that by default, all of the cell zones will be exported. If you want to export

solution data for particular surfaces, then select them from the Surfaces list. Once you have chosen

your cells zones and/or surfaces you must select the Quantities that you want to export. When selecting

the variables, be sure to include any variable that was used to create an isosurface or clipped surface

(as described in Isosurfaces (p. ) and Clipping Surfaces (p. ), respectively); otherwise, the surface

will not be created properly if you try to read the exported state file in CFD-Post.

Specify the format of the .cdat file by selecting either Binary or ASCII from the Format list. The

advantage of the binary format is that it takes less time to load the exported data into ANSYS CFD-

Post and requires less storage space. Note that the format for the .cst will always be ASCII.

By default, Fluent will write a case file (that is, .cas) along with the CDAT for CFD-Post and EnSight

files. If you do not want such a case file for any reason (for example., to improve I/O performance or

save disc space), disable the Write Case File option. Disabling this option is only recommended if you

are performing multiple export operations for a case file that is not changing.

Click the Write... button to save the files, using the Select File dialog box. A .cdat file is written,

containing the specified variable data for the specified cell zones and all of the boundary zones. A

state file (that is, .cst) is also written, which contains the following surfaces that you created in Fluent

for postprocessing: point surfaces, line surfaces, plane surfaces, isosurfaces, and clipped surfaces (see

Creating Surfaces and Cell Registers for Displaying and Reporting Data (p. )).

Note

Imprinted surfaces defined in ANSYS Fluent are not available for postprocessing in ANSYS

CFD-Post.

Important

When you read the .cdat file into ANSYS CFD-Post, the application will attempt to read

in the case file that produced the data by looking in the folder for a .cas file with the

same prefix. If the case file is not in that folder (e.g., if you disabled the Write Case File

option when exporting), ANSYS CFD-Post will prompt you to specify the appropriate case

file.

Important

Before loading the .cst file into ANSYS CFD-Post, make sure that the .cas and .cdat

files are already loaded for the session.

details.

Select CGNS from the File Type drop-down list and specify the scalars you want in the Quantities

list.

Select the Location from which the values of scalar functions are to be taken. If you specify the data

Location as Node, then the data values at the node points are exported. If you choose Cell Center,

then the data values from the cell centers are exported. For boundary faces, it is the face center values

that are exported when the Cell Center option is selected.

Click the Write... button to save the file, using the Select File dialog box. CGNS (CFD general notation

system) is a single file (for example, file.cgns) containing coordinates, connectivity, zone information,

velocity, and selected scalars.

Important

ANSYS Fluent supports exporting polyhedral data to CGNS.

details.

details.

Select Data Explorer from the File Type drop-down list and choose the surface(s) for which you want

to write data in the Surfaces list. If no surfaces are selected, the entire domain is exported. Also specify

the scalars you want in the Quantities list.

Important

When you are exporting data for Data Explorer, EnSight Case Gold, or I-deas Universal and

the reference zone is not a stationary zone, the data in the velocity fields is exported by

default as velocities relative to the motion specification of that zone. This data is always

exported, even if you do not choose to export any scalars. Any velocities that you select to

export as scalars in the Quantities list (for example, X Velocity, Y Velocity, Radial Velocity,

and so on) are exported as absolute velocities. For all other types of exported files, the ve-

locities exported by default are absolute velocities.

Click the Write... button to save the file, using the Select File dialog box. A single file (for example,

file.dx) is exported, containing coordinate, connectivity, velocity, and specified function data.

details.

When exporting to EnSight, you can choose to export the data associated with a single data file, or

you can export the data associated with multiple files that were generated by a transient solution.

To export the solution data from a single data file, read in the case and data file and open the Export dialog

box.

Then perform the following steps in the Export dialog box:

. Select EnSight Case Gold from the File Type drop-down list.

. Select the Location from which the values of scalar functions are to be taken. If you specify the data

. Specify the format of the file by selecting either Binary or ASCII from the Format list.The advantage

of the binary format is that it takes less time to load the exported files into EnSight.

. (optional) Select the Cell Zones from which you want data exported (you must select at least one zone).

By default, all of the cell zones are selected.

. (optional) Select the Interior Zone Surfaces from which you want data exported. By default, the data

being exported is taken from the entire ANSYS Fluent domain.The Interior Zone Surfaces selection

list allows you to also specify that the data be taken from selected zone surfaces whose Type is identified

as interior in the Boundary Conditions task page.

Note

Data on user defined/created surfaces is not available for export to EnSight Case Gold

file format.

. Select the scalars you want to write from the Quantities selection list.

. Click the Write... button to open the Select File dialog box, which you can use to save a file that contains

the specified variable data for the specified cell zones, the specified interior zone surfaces, and all of

the boundary zones.

To export solution data associated with multiple files that were generated by a transient solution, you must

first make sure that the following criteria are met:

– All of the relevant case and data files must be in the working folder.

– The data files must be separated by a consistent number of time steps.

Next, enter the following text command in the console:

file → transient-export → ensight-gold-from-existing-files

Then, enter responses to the following prompts in the console:

. EnSight Case Gold file name

Enter the name you want assigned to the exported files.

. Case / Data file selection by base name?

Enter yes if the case and data files share a “base name” (that is, a common initial string of

characters). The alphanumeric order of the full names must correspond to the order in which

the files were created. You will then be prompted to enter the base name at the Case / Data

file base name prompt that follows. For example, with a set of files named elbow-,

elbow-, elbow-, and so on, enter elbow- for the base name.

Enter no if you have created an ASCII file in the working folder that lists the names of the data

files in order of when they were created. The file should list one data file name per line. You will

then be prompted to enter the name of this file at the Provide the file name which

contains the data file names prompt that follows. Note that you must include the

file extension if any in your entry at the prompt.

. Specify Skip Value

Enter an integer value to specify the number of files you want to skip in between exporting files

from the sequence. For example, enter  to export every other file, enter  to export every third

file, and so on.

. Cell-Centered?

Enter yes if you want to export the data values from the cell centers (or face center values, for

boundary faces).

Enter no if you want to export the data values from the node points.

. Write separate file for each time step for each variable?

Enter yes if you want separate EnSight Case Gold files written for each time step. Otherwise, all

of the data for the .scl1 and .vel files will be combined into a single file for each.

. Write in binary format?

Enter yes to write the files in binary format. Otherwise, they will be written in ASCII format. The

advantage of the binary format is that it takes less time to load the exported files into EnSight.

. Specify Data File Frequency

Enter the number of time steps between the data files being exported.

. Separate case file for each time step?

Enter no if all the data files were generated from the same case file (that is, the simulation involved

a static mesh). Note that the name of the case file must be the same (not including the extension)

as the name of the first data file in the sequence.

Enter yes if the data files were generated from the different case files (that is, the simulation

involved a sliding or dynamic mesh). Note that the names of the case files must be the same

(not including the extension) as the names of the corresponding data files.

. Read the case file?

Enter no if the first (or only, for a static mesh) case file is already in memory.

Enter yes if the first (or only, for a static mesh) case file is not already in memory.

. cell zone id/name()

Enter the name or ID of any cell zone from which you want data exported. By default, the data

being exported is taken from the entire ANSYS Fluent domain. After you specify the first cell

zone, you will be prompted to specify the second one, and so on, until you press Enter without

typing any characters.

. Interior Zone Surfaces()

Enter the name of any interior zone surface from which you want data exported. By default, the

data being exported is taken from the entire ANSYS Fluent domain. This prompt allows you to

also specify that the data be taken from selected zone surfaces whose Type is identified as in-

terior in the Boundary Conditions task page. After you specify the first interior zone surface,

you will be prompted to specify the second one, and so on, until you press Enter without typing

any characters.

. EnSight Case Gold scalar() else q to continue

Enter in the first scalar quantity you want exported. You can press the Enter key to print a list

of available scalar quantities in the console. After you enter the first quantity, you will be

prompted to enter the second quantity, and so on, until you enter q. The EnSight Case Gold files

will then be written.

When exporting to EnSight Case Gold, files will be created with the following four formats:

A geometry file (for example, file.geo) containing the coordinates and connectivity information.

A velocity file (for example, file.vel) containing the velocity.

A scalar file (for example, file.scl1) for each selected variable or function.

An EnSight case file (for example, file.encas) that contains details about the other exported files.

Important

For non-stationary reference zones, all the velocities are exported to EnSight as velocities relative

to the selected reference zone. See the informational note in Data Explorer Files (p. ) for further

details.

ANSYS Fluent supports exporting polyhedral data to EnSight.

You also have the option of exporting data at specified intervals during a transient calculation through

the Automatic Export dialog box. For details, see Exporting Data During a Transient Calculation (p. ).

This file type is valid only for triangular and tetrahedral meshes. Select FAST from the File Type drop-

down list and select the scalars you want to write in the Quantities list.

Click the Write... button to save the file for the specified function(s), using the Select File dialog box.

The following files are written:

A mesh file in extended Plot3D format containing coordinates and connectivity.

A velocity file containing the velocity.

A scalar file for each selected variable or function.

details.

This file type is valid only for triangular and tetrahedral meshes. Select FAST Solution from the File

Type drop-down list and click the Write... button. A single file is written containing density, velocity,

and total energy data.

details.

Select Fieldview Unstructured from the File Type drop-down list. Next, specify the cell zones and

surfaces from which you want data exported by making selections in the Cell Zones or Surfaces lists

(you must select at least one zone or surface); note that by default, all of the cell zones will be exported.

Then select the scalars you want to write in the Quantities list. Finally, click the Write... button to

open the Select File dialog box, which you can use to save a file that contains the specified function(s)

for the specified cell zones and associated boundary zones or surfaces.

A binary file (for example, file.fvuns) containing coordinate and connectivity information and specified

scalar function data. In parallel, each partition writes to this file with a grid for each cell zone or surface

that is exported.This allows parallel postprocessing in FieldView.

A regions file (for example, file.fvuns.fvreg) containing information about the cell zones or surfaces

and the frame of reference. It also includes information about which grids make up the various cell zones

or surfaces.

The cell zone and surface information includes the names of the cell zones/surfaces along with the

mesh numbers. For the moving frame of reference, the regions file contains information about the

origin, the axis of rotation and the rotation speed. Volume data is written using the absolute frame of

reference.

If you are running multiple steady-state solutions on the same mesh, you can export only the data

files and avoid the repeated writing of the mesh file by using the following TUI command for surfaces

and cell zones:

file/export/fieldview-unstruct-data file_name ( list_of_surfaces ) ( list_of_zones )

list_of_scalars q

where

file_name specifies the name (without the extension) of the file that you want to write.

list_of_surfaces specifies the list of surfaces (separated by spaces, that is, no commas) from which you want

data exported. If you want to specify all of the surfaces, enter * within the parentheses.

list_of_zones specifies the list of cell zones (separated by spaces, that is, no commas) from which you want

data exported. If you want to specify all of the cell zones, enter * within the parentheses.

list_of_scalars specifies the list of cell functions (separated by spaces, that is, no commas) that you want to

write to the exported file.The q input terminates the list. For example, the input x-velocity cell-

zone q will select  velocity and the cell volume.

To export only the data files for surfaces, use the following TUI command:

file/export/fieldview-unstruct-surfaces  file_name ( list_of_surfaces ) list_of_scalars

q

where

specifies that you want to write a Fieldview unstructured results only file.

write to the exported file.The q input terminates the list. For example, the input x-velocity q will select

only the  velocity.

details.

Important

If you intend to export data to I-deas, ensure that the mesh does not contain pyramidal

elements, as these are currently not supported by I-deas.

Select I-deas Universal from the File Type drop-down list. Select the surface(s) for which you want

to write data in the Surfaces list. If no surfaces are selected, the entire domain is exported. You can

specify which scalars you want in the Quantities list.

You have the option of selecting loads to be included in the exported file. When the Energy Equation

is enabled in the Energy Dialog Box (p. ), you can choose the loads based on the kind of finite element

analysis you intend to undertake. By selecting Structural in the Analysis list, you can select the following

Structural Loads: Force, Pressure, and Temperature. By selecting Thermal in the Analysis list, you

can select the following Thermal Loads: Temperature, Heat Flux, and Heat Trans Coeff.

These loads have the following limitations:

Important

For non-stationary reference zones, all the velocities are exported to I-deas Universal as ve-

locities relative to the selected reference zone. See the informational note in Data Ex-

plorer Files (p. ) for further details.

Click the Write... button to save the file, using the Select File dialog box. A single file is written con-

taining coordinates, connectivity, optional loads, zone groups, velocity, and selected scalars.

details.

Select NASTRAN from the File Type drop-down list. Select the surface(s) containing the data you want

details.

to export in the Surfaces list. If you do not select any surfaces, the entire domain is exported. You can

Note

If you are exporting data on a polyhedral mesh, only zone surfaces will be available for se-

lection (no volumetric data or user-defined surfaces).

These loads have the following limitations :

file.bdf) is written containing coordinates, connectivity, optional loads, zone groups, and velocity.

Pressure is written as PLOAD4, and heat flux is written as QHBDYE data. If you select wall zones in the

Surfaces list, nodal forces are written for the walls. When data is written for the heat transfer coefficient,

it is based on the wall faces rather than the nodes.

Automatic Export dialog box. For details, see Exporting Data During a Transient Calculation (p. ).

Select PATRAN from the File Type drop-down list. Select the surface(s) for which you want to write

data in the Surfaces list. If you do not select any surfaces, the entire domain is exported. You can

Click the Write... button to save the file, using the Select File dialog box. A neutral file (for example,

file.out) is written containing coordinates, connectivity, optional loads, zone groups, velocity, and

selected scalars. Pressure is written as a distributed load. If wall zones are selected in the Surfaces list,

nodal forces are written for the walls. The PATRAN result template file (for example, file.res_tmpl)

is written, which lists the scalars present in the nodal result file (for example, file.rst).

The option to export a TAITherm file type is available only when the Energy Equation is enabled in

the Energy Dialog Box (p. ). Select TAITherm from the File Type drop-down list and select the

surface(s) for which you want to write data in the Surfaces list. If no surfaces are selected, the entire

domain is exported. If the mesh contains polyhedral cells, ANSYS Fluent will export only boundary

data. No volume data will be exported.

Select the method of writing the heat transfer coefficient (Heat Transfer Coefficient), which can be

Flux Based or, if a turbulence model is enabled, Wall Function based. The flux-based heat transfer

coefficient is calculated using Equation . (p. ). If no turbulence model is enabled, the wall-

function based heat transfer coefficient is calculated as

, where  is the thermal conductivity, and

is the cell height of the wall-adjacent cell.

Click the Write... button to save the file, using the Select File dialog box. A PATRAN neutral file (for

example, file.neu) is written containing element velocity components (that is, the element that is

just touching the wall), heat transfer coefficients, and temperatures of the wall for any selected wall

surface. If the wall is one-sided, the data is written for one side of the wall. If the wall is two-sided (a

wall-wall shadow pair), the values are written only for the original wall face, not for the shadow face

(which is a duplicate).

details.

Note

If no turbulence model is enabled, the Wall Function based Heat Transfer Coefficient is

equal to k/h, where k is the thermal conductivity, and h is the cell height of the wall-adjacent

cell.

Select Tecplot from the File Type drop-down list and choose the surface(s) for which you want to

write data in the Surfaces list. If no surfaces are selected, the data is written for the entire domain.

Select the variable(s) for which data is to be saved in the Quantities list.

taining the coordinates and scalar functions in the appropriate tabular format.

Important

The utility fe2ram can import Tecplot files only in FEPOINT format.

If you intend to postprocess ANSYS Fluent data with Tecplot, you can either export data from

ANSYS Fluent and import it into Tecplot, or use the Tecplot ANSYS Fluent Data Loader included

with your Tecplot distribution.The data loader reads native ANSYS Fluent case and data files

directly. If you are interested in this option, contact Tecplot, Inc. for assistance or visit

www.tecplot.com.

details.

Particle history data can be exported for steady-state solutions or for single transient particle steps by

selecting the Particle History Data... option under the File/Export ribbon tab and performing the

steps described in this section. For details about exporting particle history data automatically during

transient simulations, see Creating Automatic Export Definitions for Transient Particle History Data (p. ).

File → Export → Particle History Data...

Exporting Steady-State Particle History Data

Figure . : The Export Particle History Data Dialog Box

. Specify the File Type you want to export by selecting one of the following:

CFD-Post for the CFD-Post compatible format

FieldView for the FIELDVIEW format

EnSight for the EnSight format

Geometry for the .ibl format (not available when Unsteady Particle Tracking is enabled in the Discrete

Phase Model dialog box)

Important

If you plan to export particle data to EnSight, you should first verify that you have already

written the files associated with the EnSight Case Gold file type by using the File/Ex-

port/Solution Data... ribbon tab option (see EnSight Case Gold Files (p. )).

Select the predefined injections that are the source of the particles from the Injections selection

list. See Creating and Modifying Injections (p. ) for details about creating injections.

. Select the particle variables contained in the export file by clicking the Exported Particle Variables...

button and selecting the variables appearing in the Reporting Variables dialog box (Figure . :The

Reporting Variables Dialog Box (p. )), as described in Reporting of Current Positions for Unsteady

Tracking (p. ). Note that although the variable Particle Residence Time does not appear in the Available

Particle Variables selection list, it is always exported.

. If you have added the Color by variable in the Reporting Variables dialog box, select an appropriate

category and variable under Quantity for the particle data to be exported.

. If your exported particle history file is too large to postprocess because there are too many tracks or particles

written to the file, you can reduce the number of particle tracks by increasing the Skip value.

. To control the exported file size, the number of points of the particle trajectories can be reduced using the

Coarsen value.This is only valid for steady-state particle trajectories.

. Enter the name (and folder path, if you do not want it to be written in the current folder) for the exported

particle data file in the Particle File Name text box. Alternatively, you can specify it through the Select

File dialog box, which is opened by clicking the Browse... button.

. If you selected EnSight under File Type, you should specify the EnSight Encas File Name. Use the Browse...

button to select the .encas file that was created when you exported the file with the File/Export/Solution

Data... ribbon tab option.The selected file will be modified and renamed as a new file that contains inform-

ation about all of the related particle files that are generated during the export process (including geometry,

velocity, scalars, particle and particle scalar files).

The name of the new file will be the root of the original file with .new appended to it (for example,

if test.encas is selected, a file named test.new.encas will be written). It is this new file that

should be read into EnSight. If you do not specify a EnSight Encas File Name, then you must create

an appropriate .encas file manually.

. If you selected EnSight under File Type, and you are exporting steady-state particle tracks, enter the

Number of Particle Time Steps.

. Click Write to export the particle history data. If you selected EnSight under File Type, data files will be

written in both .mpg and .mscl formats.

. Click Close to close the dialog box.

Before you run a transient flow solution, you can set up the case file so that solution data and particle

history data is exported as the calculation progresses. This is accomplished by creating automatic export

definitions using the Calculation Activities Task Page (p. ) (Figure . : The Calculation Activities Task

Page (p. )), as described in the following sections.

Exporting Data During a Transient Calculation

Figure . : The Calculation Activities Task Page

The names of the automatic export definitions you create are displayed in the Automatic Export selection

list, along with the format in which it will be exported. You can edit or delete the definition by selecting

a definition in the list and clicking the Edit... or Delete button,.

... Creating Automatic Export Definitions for Solution Data

... Creating Automatic Export Definitions for Transient Particle History Data

To create an automatic export definition for solution data, begin by making sure that Transient is se-

lected for Time in the General Task Page (p. ). Next, click the Create button under the Automatic

Export selection list in the Calculation Activities task page (a drop-down list will appear). Select

Solution Data Export... from the drop-down list to open the Automatic Export dialog box (Fig-

ure . : The Automatic Export Dialog Box (p. )).

Figure . : The Automatic Export Dialog Box

Then perform the following steps:

. Enter a name for the automatic export definition in the Name text box.This is the name that will be dis-

played in the Automatic Export selection list in the Calculation Activities task page.

. Define the data to be exported by making selections in the relevant group boxes and selection lists: File

Type, Cell Zones, Surfaces, Interior Zone Surfaces, Quantities, Analysis, Structural Loads, Thermal

Loads, Location, Delimiter, Format, and Heat Transfer Coefficient. See ABAQUS Files (p. ) –

Tecplot Files (p. ) for details about the specific options available for the various file types.

. Set the frequency at which the solution data will be exported during the calculation using the Export

Data Every field and specify whether you want the save rate based on Time Steps or Flow Time.

. If you selected EnSight Case Gold from the File Type drop-down list, the Separate Files for Each Time

Step option allows you to specify that separate files are written at the prescribed time steps.This option

is enabled by default and is the recommended practice, as it ensures that all of the data is not lost if there

is a disruption to the calculation (for example, from a network failure) before it is complete. If you choose

to disable this option, all of the data for the .scl1 and .vel files will be combined into a single file for

each.

. If you selected CDAT for CFD-Post and EnSight from the File Type drop-down list, by default ANSYS

Fluent will save a case (.cas) file with every .cdat file (that is, at the specified Frequency).You can

change the criteria for when case files are saved by disabling the Write Case File Every Time option;

then, ANSYS Fluent will save case files according to the settings specified by the following text command:

file → transient-export → settings → cdat-for-cfd-post-&-ensight

By default, the cdat-for-cfd-post-&-ensight text command is set to save a case file only

if ANSYS Fluent detects that the mesh or case file has been modified.

Note that regardless of the settings, only a single .cst file will be written when exporting during

a transient calculation.

For more information about the CDAT for CFD-Post and EnSight file type, refer to CDAT for CFD-

Post and EnSight (p. ).

. Specify how the exported files will be named. Every file saved will begin with the characters entered in

the File Name text box (note that a file extension is not necessary).You can specify a folder path if you

do not want it written in the current folder.The File Name can also be specified through the Select File

dialog box, which is opened by clicking the Browse... button.

Next, make a selection in the Append File Name with drop-down list, to specify that the File

Name be followed by either the time step or flow time at which it was saved. Note that this selection

is not available when exporting to EnSight. When EnSight Case Gold is selected from the File

Type drop-down list, the time step is always appended if the Separate Files for Each Time Step

option is enabled; otherwise, no digits are appended.

When appending the file name with the flow time, you can specify the number of decimal places

that will be used by making an entry in the Decimal Places in File Name text box. By default, six

decimal places will be used.

. Click OK to save the settings for the automatic export definition.

Important

If the files that are exported during multiple transient simulations are to be used as a set, you

should run all of the simulations on the same platform, using the same number of processors.

This ensures that all of the files are compatible with each other.

Note

If you selected EnSight Case Gold from the File Type drop-down list, ANSYS

Fluent does not support exporting data files to EnSight during a transient cal-

Note

culation in which a new cell zone or surface is created after the calculation

has begun (as can be the case for an in-cylinder simulation, for example).

... Creating Automatic Export Definitions for Transient Particle History

Data

To create an automatic export definition for particle history data, begin by making sure that Unsteady

Particle Tracking is selected in the Discrete Phase Model dialog box. Next, click the Create button

under the Automatic Export selection list in the Calculation Activities task page (a drop-down list

will appear). Select Particle History Data Export... from the drop-down list to open the Automatic

Particle History Data Export dialog box (Figure . : The Automatic Particle History Data Export Dialog

Box (p. )).

Figure . : The Automatic Particle History Data Export Dialog Box

played in the Automatic Export selection list in the Calculation Activities task page. Make sure that the

chosen name is not already used for another Automatic Export.

. Choose the File Type you want to export by selecting one of the following:

Important

If you plan to export particle data to EnSight, you should first set up an automatic export

definition so that solution data is also exported to EnSight during this calculation (see

Creating Automatic Export Definitions for Solution Data (p. )). As described in the

steps that follow, some of the settings must correspond between the two automatic

export definitions.

. Select the predefined injections that are the source of the particles from the Injections selection list. See

Creating and Modifying Injections (p. ) for details about creating injections.

. Set the Frequency at which the particle history data will be exported during the calculation. If you enter

in the Frequency text box, for example, a file will be written after every  time steps for transient

flow cases or  DPM Iterations for steady flow cases.

. If your exported particle history file is too large to postprocess because there are too many tracks or

particles written to the file, you can reduce the number of particle tracks by increasing the Skip value.

. If you selected EnSight Case Gold for the File Type, the Separate Files for Each Time Step option allows

you to specify that separate files are written at the prescribed time steps.This option is enabled by default

and is the recommended practice, as it ensures that all of the data is not lost if there is a disruption to the

calculation (for example, from a network failure) before it is complete. If you choose to disable this option,

all of the data for the .mscl and .mpg files will be combined into a single file for each.

Important

The setting for the Separate Files for Each Time Step option should be the same (that

is, enabled or disabled) as that of the automatic export definition you set up to export

solution data to EnSight during this calculation. For details, see Creating Automatic Export

Definitions for Solution Data (p. ).

File dialog box, which is opened by clicking the Browse... button. Make sure the file name is different

from other existing Automatic Export definitions to avoid overwriting data.

If you selected FieldView under File Type, you can write particle history data for each time step

to separate files by including the character string %t in the particle file name. At the time of export,

Fluent will substitute %t with the current time step. The saved files can be processed by FieldView

or newer.

. If you selected EnSight under File Type, you should specify the EnSight Encas File Name. Enter the same

name (and folder path, if necessary) that you entered in the File Name text box when you set up the

automatic export definition for exporting solution data to EnSight during this calculation. (For details, see

Creating Automatic Export Definitions for Solution Data (p. )).The .encas file created during the

solution data export will be modified and renamed as a new file that contains information about all of

the related particle files that are generated after every time step during the export process (including

geometry, velocity, scalars, particle and particle scalar files).The name of the new file will be the root of

the original .encas file with .new appended to it (for example, if the solution data export creates

test.encas, a file named test.new.encas will be written for the particle data export). It is this new

file that should be read into EnSight.

Important

If you do not specify an EnSight Encas File Name, you will have to manually create an

appropriate .encas file.

The particle data will be exported as it is generated during the transient calculation. If you selected

EnSight under File Type, data files will be written in both .mpg and .mscl formats.

You can use the Export to CFD-Post dialog box (Figure . : The Export to CFD-Post Dialog Box (p. ))

to export the results from cell zones and/or surfaces to files that are compatible with ANSYS CFD-Post

(and EnSight).

For instructions on exporting variables in ANSYS CFD-Post compatible file format (.cdat) using this

dialog box, see CDAT for CFD-Post and EnSight (p. ).

File → Export to CFD-Post...

Figure . : The Export to CFD-Post Dialog Box

Exporting to ANSYS CFD-Post

By default, the Open CFD-Post option is enabled so that the following actions will occur after the files

are exported:

. A CFD-Post session opens automatically.

. The case and .cdat files are loaded in CFD-Post.

. CFD-Post displays the results.

If you disable the Open CFD-Post option, you can open CFD-Post manually and use the Load Results

item in the File drop-down menu to load the results files. For more information about this feature in

CFD-Post, see the separate ANSYS CFD-Post manual.

Note

When exporting to CFD-Post, Fluent only saves a new case file if the mesh or case has changed

since the last time the case file was saved, which conserves storage space.

CFD-Post may have difficulty reading transient cases that have changing mesh topology and/or

zones added/removed during the simulation.

Using the EnSight Parallel  option in the Export dialog box you can save Fluent solution case and

data files for postprocessing in ANSYS EnSight Enterprise (EnSight in parallel).

To setup parallel EnSight export in Fluent:

. Ensure that you are running Fluent in parallel. This functionality is only available when Fluent is running in

parallel.

. Open the Export dialog box.

. Select EnSight Case Gold from the File Type drop-down.

. Select either Node or Cell Center for the Location where the data will be written.

. Select the Format for how the data will be saved.

. Enable EnSight Parallel.

. Select either the Cell Zones or Surfaces that you want to export.

. Select the Quantities that you want to export.

. Click Write... to specify the location where the data will be saved.

Note that you can also setup for automatic exporting of solution data using the same steps as described

above but using the Automatic Export Dialog Box (p. ).

Important

You can either export solution data from Cell Zones or Surfaces, but you cannot do both

at once.

You can manage your solution files effectively and efficiently using the Solution Files dialog box. Here,

you can select previously saved files created using the Autosave dialog box and read or delete them.

File → Solution Files...

Managing Solution Files

Figure . : The Solution Files Dialog Box

The Solution Files dialog box (Figure . : The Solution Files Dialog Box (p. )) lists all of the solution

files that have been automatically saved. They are listed by iteration number or time step/flow time.

For the file that is currently read in, the status of current will appear in the Solution Files at list. You

can make any of the files in the list current by clicking the Read button. Note that if more than one file

is selected, the Read button is disabled. When an earlier solution is made current, the solution files that

were generated for a later iteration/time step will be removed from this list when the calculation con-

tinues.

You can delete solution files by selecting an entry in the list and clicking Delete. Note that a currently

loaded solution file cannot be deleted, however multiple (non-current) files can be selected and deleted.

If multiple files are selected and one of those files is a currently loaded solution file, clicking Delete will

result in the current solution file being skipped.

You can click the File Names... button to obtain information about the solution files and the path of

the associated files.

When running Fluent under Workbench, you can recover the latest case and data files from the system

folder (<project name>\dp0\FFF\Fluent\ for analysis system and <project name>\dp0\

FLU \Fluent\ for component system) by clicking Recover Missing Solution... The recovered files

will appear in the Solution Files at list. You can use this option when the latest matching/compatible

case and data files are missing from the Solution Files at list.

The Solution Files dialog box is particularly useful for reading in files that were saved during the

autosave session, since case and data files may not necessarily have the same file name.

ANSYS Fluent can interpolate solution data for a given geometry from one mesh to another, allowing

you to compute a solution using one mesh (for example, hexahedral) and then change to another mesh

(for example, hybrid) and continue the calculation using the first solution as a starting point.

Important

ANSYS Fluent does zeroth-order interpolation for interpolating the solution data from one

mesh to another.

... Performing Mesh-to-Mesh Solution Interpolation

... Format of the Interpolation File

The procedure for mesh-to-mesh solution interpolation is as follows:

. Set up the model and calculate a solution on the initial mesh.

. Write an interpolation file for the solution data to be interpolated onto the new mesh, using the Interpolate

Data dialog box (Figure . :The Interpolate Data Dialog Box (p. )).

File → Interpolate...

Figure . : The Interpolate Data Dialog Box

a.

Under Options, select Write Data.

Mesh-to-Mesh Solution Interpolation

b. In the Cell Zones selection list, select the cell zones for which you want to save data to be interpolated.

Note

If your case includes both fluid and solid zones, write the data for the fluid zones

and the data for the solid zones to separate files.

c.

Select the variable(s) for which you want to interpolate data in the Fields selection list. All ANSYS

Fluent solution variables are available for interpolation.

d. Select the Binary File check box if you want a binary interpolation file to be generated.

Note

Writing a binary interpolation file is significantly faster and requires less memory

than writing a text file.

e. Click Write... and specify the interpolation file name in the resulting Select File dialog box.The file

format is described in Format of the Interpolation File (p. ).

. Set up a new case.

a.

Read in the new mesh, using the appropriate ribbon tab item (File/Read/ or File/Import/).

b. Define the appropriate models.

Important

Enable all of the models that were enabled in the original case. For example, if the

energy equation was enabled in the original case and you forget to enable it in the

new case, the temperature data in the interpolation file will not be interpolated.

c.

c.

Define the boundary conditions, material properties, and so on.

Important

An alternative way to set up the new case is to save the boundary conditions from the

original model using the write-settings text command, and then read in those

boundary conditions with the new mesh using the read-settings text command.

See Reading and Writing Boundary Conditions (p. ) for further details.

. Read in the data to be interpolated.

a.

Under Options, select Read and Interpolate.

b. In the Cell Zones list, select the cell zones for which you want to read and interpolate data.

If the solution has not been initialized, computed, or read, all zones in the Cell Zones list are

selected by default, to ensure that no zone remains without data after the interpolation. If all

zones already have data (from initialization or a previously computed or read solution), select

a subset of the Cell Zones to read and interpolate data onto a specific zone (or zones).

c.

Click the Read... button and specify the interpolation file name in the resulting Select File dialog box.

Important

If your case includes both fluid and solid zones, the two sets of data are saved to separate

files. Hence perform these steps twice, once to interpolate the data for the fluid zones

and once to interpolate the data for the solid zones.

. Reduce the under-relaxation factors and calculate on the new mesh for a few iterations to avoid sudden

changes due to any imbalance of fluxes after interpolation.Then increase the under-relaxation factors

and compute a solution on the new mesh.

An example of an interpolation file is shown below:

pressure

(-.

.

...

The format of the interpolation file is as follows:

The first line is the interpolation file version. It is  for files generated using ANSYS Fluent . through

.,  for text files generated using ANSYS Fluent .,  for binary files generated using single precision

ANSYS Fluent ., and  for files generated using double precision ANSYS Fluent ..

The second line is the dimension ( or ).

The third line is the total number of points.

The fourth line is the total number of fields (temperature, pressure, and so on) included.

Starting at the fifth line is a list of field names.To see a complete list of the field names used by ANSYS

Fluent, enter the display/contour text command and view the available choices by pressing Enter at

the contours of> prompt.The list depends on the models turned on.

After the field names is a section for each list of ,

, and (in 3D)  coordinates for all the data points.

At the end is a section for each list of the field values at all the points in the same order as their names.The

number of coordinate and field points should match the number given in line .

For version  interpolation files, the sections are bounded by “(” and “)”.

For version  and  interpolation files, the sections are bounded by “(” and “\nEnd of Binary Section )”.

The delimiters help skip a section if the associated model is not enabled.With version  interpolation files

(where the delimiters do not exist), sections may not be skipped properly if the size of the field cannot be

determined without enabling the associated model.This may result in incorrect interpolation of the sub-

sequent field variables.

Important

An interpolation file written with ANSYS Fluent . and above is not readable in prior

versions of ANSYS Fluent.

ANSYS Fluent allows you to map variables (for example, temperature, pressure) from the cell or face

zones of an ANSYS Fluent simulation onto locations associated with a finite element analysis (FEA) mesh.

The results are written to a file for inclusion into an FEA simulation. During this process, both the ori-

ginal and the new mesh can be viewed simultaneously. ANSYS Fluent maps the data using zeroth-order

interpolation, and can write the output file in a variety of formats.

This capability is useful when solving fluid-structure interaction (FSI) problems, and allows you to perform

further analysis on the solid portion of your model using FEA software. Mapping the data may be

preferable to simply exporting the ANSYS Fluent data file (as described in Exporting Solution Data (p. )),

since the meshes used in CFD analysis are typically finer than those used in finite element analysis.

... FEA File Formats

... Using the FSI Mapping Dialog Boxes

The FEA software types that are compatible with ANSYS Fluent’s FSI mapping capability include ABAQUS,

I-deas, ANSYS, NASTRAN, and PATRAN. For details about the kinds of files that can be read or written

during this process, see Table . : FEA File Extensions for FSI Mapping (p. ).

Table . : FEA File Extensions for FSI Mapping

Output File

Input File

Type

.inp

.inp

ABAQUS

.unv

.unv

I-deas

.cdb

.cdb, .neu

ANSYS

.bdf

.bdf

NASTRAN

.out

.neu, .out, .pat

PATRAN

To begin the process of mapping ANSYS Fluent data, you must first create a mesh file that can be used

as the input file in the steps that follow. The resolution of the mesh should be appropriate for your

eventual finite element analysis. You are free to use the method and preprocessor of your choice in

the creation of this file, but the end result must correspond to one of the entries in the Input File

column of Table . : FEA File Extensions for FSI Mapping (p. ).

When creating the input file, note the following:

While the input file may be scaled when it is read into ANSYS Fluent, the volumes or surfaces on which the

data is to be mapped must otherwise be spatially coincident with their counterparts in the ANSYS Fluent sim-

ulation.

ANSYS Fluent can map volume and surface data only for 3D cases; data mapping is not supported for 2D

cases since data mapping for edges is not supported.

The input file can be only a portion of the overall FEA model (that is, you can exclude the parts of the

model on which you are not mapping ANSYS Fluent data).When this is the case, note that the numbering

of the nodes and elements in the input file must match the numbering of the nodes and elements in the

complete file you will use for your finite element analysis.

Next, read a case file in ANSYS Fluent and make sure data is available for mapping, either by running

the calculation or by reading a data file.

Finally, perform the following steps to generate an output file in which the ANSYS Fluent data has

been mapped to the mesh of the input file:

. Open the ANSYS Fluent dialog box that is appropriate for the zones from which the data is to be taken.

If the data you are mapping is from a volume (for example, the cell zone of a solid region), open the

Volume FSI Mapping dialog box using the File/FSI Mapping/Volume... ribbon tab item (Figure . :The

Volume FSI Mapping Dialog Box for Cell Zone Data (p. )). If instead the data is from a surface (for example,

a face boundary zone), open the Surface FSI Mapping dialog box using the File/FSI Mapping/Surface...

ribbon tab item (Figure . :The Surface FSI Mapping Dialog Box for Face Zone Data (p. )).

File → FSI Mapping → Volume...

or

File → FSI Mapping → Surface...

Mapping Data for Fluid-Structure Interaction (FSI) Applications

Figure . : The Volume FSI Mapping Dialog Box for Cell Zone Data

Figure . : The Surface FSI Mapping Dialog Box for Face Zone Data

. Specify the parameters of the input file and read it into ANSYS Fluent.

a.

Select the format of the input file from the Type list in the Input File group box, based on the FEA

software with which it is associated.The choices include:

ABAQUS

I-deas

Mechanical APDL

NASTRAN

PATRAN

For a list of the file extensions associated with these types, see the Input File column of

Table . : FEA File Extensions for FSI Mapping (p. ).

ABAQUS

I-deas

NASTRAN

PATRAN

b. Enter the name and extension (along with the folder path, if it is not in the current folder) of the input

file in the FEA File text-entry box. Alternatively, you can specify it through the Select File dialog box,

which is opened by clicking the Browse... button.

c.

Specify the length units that were used in the creation of the input file by making a selection from

the Length Units drop-down menu.This ensures that the input file is scaled appropriately relative to

the ANSYS Fluent file.

d. Click the Read button to read the input file into memory.

Important

Note that the input file will only be held in memory until the output file is written, or

until the FSI mapping dialog box is closed.

. Display the meshes so that you can visually verify that the input file is properly scaled and aligned with

the ANSYS Fluent mesh file.

a.

Make sure that the FEA Mesh and Fluent - Mesh options are selected in the Display Options group

box. Note that you can disable either of these options if you want to examine one of the meshes inde-

pendently.

b. Click the Display button to display the meshes in the graphics window.

Important

For the ANSYS Fluent mesh, only the zones selected in the Fluent Zones group box will

be displayed—in this case, the default selections. If the default zones are not appropriate,

you should redisplay the meshes after you make your zone selections in a later step.

. Specify the type of data variables to be mapped.

a.

Select either Structural or Thermal in the Analysis group box.Your selection should reflect the kind

a.

of further analysis you intend to pursue, and will determine what variables are available for mapping.

b. Enable the variables you want to map in the Structural Loads or Thermal Loads group box.When

mapping volume data, you can enable only Temperature.When mapping surface data, you can enable

Force, Pressure, and Temperature for structural analysis, or Temperature, Heat Flux, and Heat Trans

Coeff for thermal analysis.

Important

Note that the Energy Equation must be enabled in the Energy dialog box if you want

to map temperature for a structural analysis or any variable for a thermal analysis.

. Select the zones that contain the data to be mapped in the Flluent Zones group box.You can select in-

dividual zones in the Cell Zones or Face Zones selection lists, or select all zones of a particular type in

the Zone Type selection list. If you modify the default selections, you should display the meshes again,

as described previously.

Important

Note that all wall zones in the Face Zones selection list are selected by default in the Surface

FSI Mapping dialog box, and this includes the shadow walls created for two-sided walls. If

your ANSYS Fluent file contains a wall/shadow pair (for example, separating a solid zone

from a fluid zone), you should make sure that only the correct wall or shadow of the pair is

selected.

Inlet zones do not have heat transfer coefficient data, and so any attempts to map this

combination will be ignored.

. Specify the parameters of the output file and write it.

a.

selected.

a.

Select the format of the output file from the Type list in the Output File group box, based on the

software with which you plan to perform your finite element analysis.The choices in this list are the

same as those for the input file type. Note that you can select an output file type that is different from

the input file type.

For details about the file extensions associated with the various types of output files, see the

Output File column of Table . : FEA File Extensions for FSI Mapping (p. ).

b. Enter the name (with the folder path, if appropriate) of the output file in the File Name text-entry box.

Alternatively, you can specify it through the Select File dialog box, which is opened by clicking the

Browse... button.

c.

To include additional FEA information like node/element information in the exported output file, enable

Include FEA Mesh. By default, this option is disabled and therefore, only the selected boundary con-

dition values are exported.

d. When mapping temperature for a structural analysis or any variable for a thermal analysis, make a

selection in the Temperature Units drop-down menu. Table . : Units Associated with the Temperature

Units Drop-Down List Selections (p. ) shows the units for the mapped variables, depending on the

Temperature Units selection.

Table . : Units Associated with the Temperature Units Drop-Down List Selections

Heat Flux

Temperature Units

Selection

W/

K

W/

K

K

W/

°C

W/

°C

C

BTU/

hr- °F

BTU/

hr

°F

F

Heat Flux

Selection

W/

K

W/

K

K

W/

°C

W/

°C

C

BTU/

hr- °F

BTU/

hr

°F

F

e. When mapping the heat transfer coefficient for a thermal analysis, make a selection in the HTC Type

drop-down menu to determine how the heat transfer coefficient

is calculated.

ref-temp

calculates

using Equation . (p. ), where

is the reference temperature defined in

the Reference Values Task Page (p. ). Note that this option has the same definition as the field

variable Surface Heat Transfer Coef., as described in Alphabetical Listing of Field Variables and

Their Definitions (p. ).

cell-temp

using the general form of Equation . (p. ), but defines

as the temperature

of the cell adjacent to the face.

wall-func-htc

using Equation . (p. ). Note that this option has the same definition as the

field variable Wall Func. Heat Tran. Coef., as described in Alphabetical Listing of Field Variables

and Their Definitions (p. ).

f.

Click Write to write an output file in which the ANSYS Fluent data has been mapped to the mesh of

the input file.

The input file will be released from memory when the output file is written.

Graphic window displays can be saved in various 2D and 3D formats (see Choosing the Picture File

Format (p. ) for a full listing of the supported file types). There can be slight differences between

pictures and the displayed graphics windows depending on your settings and hardware, as the pictures

may be generated using the internal software renderer while the graphics windows may use specialized

graphics hardware for optimum performance. To eliminate such differences and save these files at the

fastest rate possible, you must follow all of the following best practices:

generally the fastest method of generating a picture (since the scene is already rendered in the graphics

window), and guarantees that the picture is identical to the window.

Note

You can control the line thickness in saved images by specifying the Line width setting in

Preferences, under Save Picture Settings.

... Picture Options for PostScript Files

To set picture parameters and save picture files, use the Save Picture Dialog Box (p. ) (Figure . : The

Save Picture Dialog Box (p. )).

File → Save Picture...

Figure . : The Save Picture Dialog Box

For your convenience, this dialog box may also be opened using the Save Picture button (

) in

the standard toolbar.

The procedure for saving a picture file is as follows:

. Choose the picture file Format.

. Set the Coloring.

. Specify the File Type, if applicable.

. Define the Resolution, if applicable.

. Set the appropriate Options.

. If you are generating a window dump, specify the Window Dump Command.

. (optional) Preview the result by clicking Preview.

. Click the Save... button and enter the file name in the resulting Select File dialog box. See Automatic

Numbering of Files (p. ) for information on special features related to file name specification.

If you are not ready to save a picture but want to save the current picture settings, click the Apply

button instead of the Save... button. The applied settings become the defaults for subsequent pictures.

.... Choosing the Picture File Format

To choose the picture file format, select one of the following items in the Format list:

EPS

(Encapsulated PostScript) output is the same as PostScript output, with the addition of Adobe Document

Structuring Conventions (v2) statements. Currently, no preview bitmap is included in EPS output. Often,

programs that import EPS files use the preview bitmap to display on-screen, although the actual vector

PostScript information is used for printing (on a PostScript device).You can save EPS files in raster or

vector format.

JPEG

is a common raster file format.

PPM

output is a common raster file format.

PostScript

JPEG

PPM

is a common vector file format.You can also choose to save a PostScript file in raster format.

TIFF

PNG

HSF

is HOOPS Visualize Stream Format, a highly-compressible and streamable 2D/3D file format.

AVZ

is the free ANSYS Viewer Format, which is a 3D file format allowing you to visualize, share, collaborate,

and interactively manipulate the displayed object. For additional information on the ANSYS Viewer, refer

to ANSYS Viewer User's Guide.

Limitations for AVZ Export:

Only mesh faces (not edges) can be displayed in the ANSYS Viewer.

Contour values may be displayed incorrectly in the ANSYS Viewer, if the Node Values option was disabled

when the .avz file was saved.

Scenes containing multiple colormaps may show the colormaps overlapping when displayed in the ANSYS

Viewer.You can rearrange the colormaps by dragging and dropping them to different locations in the

graphics window (top, bottom, right) in ANSYS Fluent before saving in AVZ format to avoid this overlap

issue.

The ANSYS Viewer has a fixed size for pathline and particle track displays that may not match the exact

settings of the pathline or particle track object when it was saved in .avz format in ANSYS Fluent.

2D plots cannot be saved in .avz format, including report plots, residuals, and XY plots.

Mesh included as part of a scene may appear black, if the transparency has been modified from .

Hovering over individual vectors will not display their values in the ANSYS Viewer.This also applies for

pathline displays with the Style set to either line, point, or sphere.

The colormap type and precision displayed in the ANSYS Viewer may not match how the colormap appeared

when the .avz file was saved in ANSYS Fluent.

VRML

is a graphics interchange format that allows export of 3D geometrical entities that you can display in

the ANSYS Fluent graphics window.This format can commonly be used by VR systems and the 3D geo-

metry can be viewed and manipulated in a web-browser graphics window.

Important

Non-geometric entities such as text, titles, color bars, and orientation axis are not ex-

ported. In addition, most display or visibility characteristics set in ANSYS Fluent, such

as lighting, shading method, transparency, face and edge visibility, and outer face

culling, are not explicitly exported but are controlled by the software used to view the

VRML file.

Window Dump

(Linux systems only) selects a window dump operation for generating the picture.With this format, you

must specify the appropriate Window Dump Command.

Important

The advantage to saving the animation sequence using the HSF File option is that these

files are highly compressible and can be viewed and interacted with using a “HOOPS

Viewer” application on iOS and Android equipped devices. The “HOOPS Viewer” application

can be downloaded to iOS and Android equipped devices from the “App Store” and “Google

Play” respectively.

An advantage to saving the animation sequence using the PPM Image option is that you

can use the separate pixmap image files for the creation of a single GIF file. GIF file creation

can be done quickly with graphics tools provided by other third-party graphics packages

such as ImageMagick, that is, animate or convert. For example, if you save the PPM

files starting with the string sequence-, and you are using the ImageMagick software,

you can use the convert command with the -adjoin option to create a single GIF file

out of the sequence using the following command.

convert -adjoin sequence-2_00*.ppm sequence2.gif

.... Specifying the Color Mode

For all formats except VRML, HSF, and the window dump, specify the type of Coloring you want to

use for the picture file.

Select Color for a color-scale copy.

Select Gray Scale for a gray-scale copy.

Select Monochrome for a black-and-white copy.

Most monochrome PostScript devices render Color images in shades of gray, but to ensure that the

color ramp is rendered as a linearly-increasing gray ramp, you should select Gray Scale.

.... Choosing the File Type

When you save an EPS (Encapsulated PostScript) or PostScript file, choose one of the following under

File Type:

A Raster file defines the color of each individual pixel in the image. Raster files have a fixed resolution.

The supported raster formats are EPS, JPEG, PPM, PostScript,TIFF, and PNG.

A Vector file defines the graphics image as a combination of geometric primitives like lines, polygons,

and text.Vector files are usually scalable to any resolution.The supported vector formats include EPS,

PostScript, and VRML.

Important

For the quickest print time, you can save vector files for simple 2D displays and raster files

for complicated scenes.

Important

.... Defining the Resolution

For raster picture files (that is, JPEG, PPM, TIFF, and PNG), you can control the resolution of the picture

image by specifying the size (in pixels). Set the desired Width and Height under Resolution. If the

Width and Height are both zero, the picture is generated at the same resolution as the active

graphics window. To check the size of the active window in pixels, click Info in the Display Options

For EPS and PostScript files, specify the resolution in dots per inch (DPI) instead of setting the width

and height.

.... Picture Options

For all picture formats except VRML, HSF, and the window dump, you can control two additional

settings under Options:

Specify the orientation of the picture using the Landscape Orientation button. If this option is turned

on, the picture is made in landscape mode; otherwise, it is made in portrait mode.

Control the foreground/background color using the White Background option. If this option is enabled,

the picture is saved with a white background, and (if you are using the classic color scheme for the

graphics window) the foreground color is changed to black.

ANSYS Fluent provides options that allow you to save PostScript files that can be printed more quickly.

The following options are found in the display/set/picture/driver/ post-format text

menu:

fast-raster

enables a raster file that may be larger than the standard raster file, but will print much more quickly.

raster

enables the standard raster file.

rle-raster

menu:

raster

enables a run-length encoded raster file that is about the same size as the standard raster file, but will

print slightly more quickly.This is the default file type.

vector

enables the standard vector file.

....Window Dumps (Linux Systems Only)

If you select the Window Dump format, the program uses the specified Window Dump Command

xwd -id %w >

When the dump occurs, ANSYS Fluent automatically interprets %w to be the ID number of the active

window.

When you click the Save... button, the Select File dialog box appears. Enter the file name for the

output from the window dump (for example, myfile.xwd).

If you are planning to make an animation, save the window dumps into numbered files, using the

%n variable. To do this, use the Window Dump Command (xwd -id %w), but for the file name in

the Select File dialog box enter myfile%n.xwd. Each time a new window dump is created, the

value of %n increases by one. So there is no need to tack numbers onto the picture file names

manually.

To use the ImageMagick animate program, saving the files in MIFF format (the native ImageMagick

format) is more efficient. In such cases, use the ImageMagick tool import. Set the default Window

Dump Command enter

Click Save... to open the Select File dialog box. Specify the output format to be MIFF by using the

.miff suffix at the end of file name.

The window dump feature is both, system and graphics-driver specific. Thus the commands available

for dumping windows depends on the particular configuration.

The window dump captures the window exactly as it is displayed, including resolution, colors, trans-

parency, and so on. For this reason, all of the inputs that control these characteristics are disabled in

the Save Picture dialog box when you enable the Window Dump format. If you are using an -bit

graphics display, use one of the built-in raster drivers (for example, TIFF) to generate higher-quality

bit color output rather than dumping the -bit window.

.... Previewing the Picture Image

Before saving a picture file, you have the option of previewing what the saved image will look like.

Click Preview to open a new window that will display the graphics using the current settings. This

allows you to investigate the effects of different options interactively before saving the final, approved

picture.

By default, the information saved in a data file includes a standard set of quantities that were computed

during the calculation. These quantities are specifically suitable for postprocessing and restarting solutions

in ANSYS Fluent. If, however, you plan to postprocess the data file in an application other than ANSYS

Fluent (such as ANSYS CFD-Post) you may want to include additional quantities that are derived from

the standard quantities.

Note that some standard quantities are also listed as additional quantities. If using ANSYS CFD-Post,

where a standard quantity has a corresponding entry in the additional quantity list, the latter should

be selected. This is because ANSYS CFD-Post requires that some standard quantities are derived in a

specific form.

Note

Not all standard quantities are available in CFD-Post for postprocessing. An example of such

a quantity is Mach number.

The procedure for generating a data file with additional quantities is as follows:

. Read the case file (.cas) for your simulation.

. Initialize the solution using the Solution Initialization Task Page (p. ).

. Specify the quantities to be written in the data file, using the Data File Quantities dialog box (Fig-

ure . :The Data File Quantities Dialog Box (p. )).

Setting Data File Quantities

File → Data File Quantities...

Figure . : The Data File Quantities Dialog Box

a.

View the Standard Quantities list to see what will be saved in the data file by default. Note that you

cannot deselect any of the Standard Quantities.

b. Select the additional quantities you want saved from the Additional Quantities selection list.

c.

Click OK.

. Save the case file. Note that the data file quantities specified in the previous step will be saved as part of

the case file.

. Run the calculation and save the data file.This can be done as separate steps, or as one step if you have

selected the automatic saving of data files via the Calculation Activities Task Page (p. ).

The Data File Quantities dialog box can also be opened by clicking the Data File Quantities... button

in the Autosave Case/Data dialog box.

When starting up, ANSYS Fluent looks in your home folder for an optional file called .fluent. If it

finds the file, it loads it with the Scheme load function. This file can contain Scheme functions that

customize the code’s operation.

The .fluent file can also contain TUI commands that are executed via the Scheme function ti-menu-

load-string. For example, if the .fluent file contains

(ti-menu-load-string "file read-case test.cas")

then ANSYS Fluent will read in the case file test.cas. For more details about the function ti-menu-

load-string, see Text Menu Input from Character Strings.

Important

Another optional file, .tgrid, if present, is also loaded at start up. This file may contain

Scheme functions that customize the operation of the code in meshing mode. When both

the .fluent and .tgrid files are present, the .tgrid file will be loaded first, followed

by the .fluent file, when the solution mode is launched. Hence, the functions in the

.fluent file will take precedence over those in the .tgrid file for the solution mode.

The .fluent file is not loaded automatically when switching to solution mode from

meshing mode. You will need to load the file separately using the Scheme load function, if

needed.

The .fluent File

Chapter : Unit Systems

This chapter describes the units used in ANSYS Fluent and how you can control them. Information is

organized into the following sections:

.. Restrictions on Units

.. Units in Mesh Files

.. Built-In Unit Systems in ANSYS Fluent

.. Customizing Units

ANSYS Fluent enables you to work in any unit system, including inconsistent units. Thus, for example,

you may work in British units with heat input in Watts or you may work in SI units with length defined

in inches. This is accomplished by providing ANSYS Fluent with a correct set of conversion factors

between the units you want to use and the standard SI unit system that is used internally by the solver.

ANSYS Fluent uses these conversion factors for input and output, internally storing all parameters and

performing all calculations in SI units. Both solvers always prompt you for the units required for all di-

mensional inputs.

Units can be altered part-way through a problem setup and/or after you have completed your calculation.

If you have entered some parameters in SI units and then you switch to British, all of your previous inputs

(and the default prompts) are converted to the new unit system. If you have completed a simulation

in SI units but you would like to report the results in any other units, you can alter the unit system and

ANSYS Fluent will convert all of the problem data to the new unit system when results are displayed.

As noted above, all problem inputs and results are stored in SI units internally. This means that the

parameters stored in the case and data files are in SI units. ANSYS Fluent simply converts these values

to your unit system at the interface level.

It is important to note that the units for some inputs in ANSYS Fluent are different from the units used

for the rest of the problem setup.

You must always define the following in SI units, regardless of the unit system you are using:

– Boundary profiles (see Profiles (p. ))

– Source terms (see Defining Mass, Momentum, Energy, and Other Sources (p. ))

– Custom field functions (see Custom Field Functions (p. ))

– Data in externally-created XY plot files (see XY Plots of File Data (p. ))

– User-defined functions (See the Fluent Customization Manual for details about user-defined functions.)

If you define a material property by specifying a temperature-dependent polynomial or piecewise-polyno-

mial function, remember that temperature in the function is always in units of Kelvin or Rankine. If you are

using Celsius or Kelvin as your temperature unit, then polynomial coefficient values must be entered in

terms of Kelvin; if you are using Fahrenheit or Rankine as the temperature unit, values must be entered in

terms of Rankine. See Defining Properties Using Temperature-Dependent Functions (p. ) for information

about temperature-dependent material properties.

Some mesh generators allow you to define a set of units for the mesh dimensions. However, when you

read the mesh into ANSYS Fluent, it is always assumed that the unit of length is meters. If this is not

true, you must scale the mesh, as described in Scaling the Mesh (p. ).

ANSYS Fluent provides four built-in unit systems: British, SI, CGS, and "default", all of which can be se-

lected in the Set Units dialog box (Figure . : The Set Units Dialog Box (p. )), using the buttons under

the Set All to heading. To display the Set Units dialog box, right-click General and click Units..., under

Setup in the tree.

Setup → General

Units

Figure . : The Set Units Dialog Box

To choose the English Engineering standard for all units, click the british button; to select the Interna-

tional System of units (SI) standard for all units, click the si button; to choose the CGS (centimeter-gram-

second) standard for all units, click the cgs button; and to return to the "default" system, click the default

button. The default system of units is similar to the SI system, but uses degrees instead of radians for

angles. Clicking on one of the buttons under Set All to will immediately change the unit system. You

can then close the dialog box if you are not interested in customizing any units.

Changing the unit system in the Set Units dialog box causes all future inputs that have units to be

based on the newly selected unit system.

Unit Systems

If you would like a mixed unit system, or any unit system different from the four supplied by ANSYS

Fluent (and described in Built-In Unit Systems in ANSYS Fluent (p. )), you can use the Set Units dialog

box (Figure . : The Set Units Dialog Box (p. )) to select an available unit or specify your own unit

name and conversion factor for each quantity.

... Listing Current Units

... Changing the Units for a Quantity

... Defining a New Unit

Before customizing units for one or more quantities, you may want to list the current units. You can

do this by clicking the List button at the bottom of the Set Units dialog box. ANSYS Fluent will print

out a list (in the text window) containing all quantities and their current units, conversion factors, and

offsets.

ANSYS Fluent will enable you to modify the units for individual quantities. This is useful for problems

in which you want to use one of the built-in unit systems, but you want to change the units for one

quantity (or for a few). For example, you may want to use SI units for your problem, but the dimensions

of the geometry are given in inches. You can select the SI unit system, and then change the unit of

length from meters to inches.

To change the units for a particular quantity, you will follow these two steps:

.

Select the quantity in the Quantities list (they are arranged in alphabetical order).

.

Choose a new unit from those that are available in the Units list.

For the example cited above, you would choose length in the Quantities list, and then select in in

the Units list. The Factor will automatically be updated to show . meters/inch. (See Figure . : The

Set Units Dialog Box (p. ).) If there was a nonzero offset for the new unit, the Offset field would

also be updated. For example, if you were using SI units but wanted to define temperature in Celsius

instead of Kelvin, you would select temperature in the Quantities list and c in the Units list. The

Factor would change to , and the Offset would change to .. Once you have selected the

quantity and the new unit, no further action is needed, unless you want to change the units for another

quantity by following the same procedure.

To create a new unit to be used for a particular quantity, you will follow the procedure below:

.

In the Set Units dialog box, select the quantity in the Quantities list.

.

Click the New... button and the Define Unit dialog box (Figure . :The Define Unit Dialog Box (p. ))

will open. In this dialog box, the selected quantity will be shown in the Quantity field.

Customizing Units

Figure . : The Define Unit Dialog Box

.

Enter the name of your new unit in the Unit field, the conversion factor in the Factor field, and the offset

in the Offset field.

.

Click OK in the Define Unit dialog box, and the new unit will appear in the Set Units dialog box.

For example, if you want to use hours as the unit of time, select time in the Quantities list in the Set

Units dialog box and click the New... button. In the resulting Define Unit dialog box, enter hr for

the Unit and  for the Factor, as in Figure . : The Define Unit Dialog Box (p. ). Then click OK.

The new unit hr will appear in the Units list in the Set Units dialog box, and it will be selected.

.... Determining the Conversion Factor

The conversion factor you specify (Factor in the Define Unit dialog box) tells ANSYS Fluent the

number to multiply by to obtain the SI unit value from your customized unit value. Thus the conversion

factor should have the form SI units/custom units. For example, if you want the unit of length to be

inches, you should enter a conversion factor of . meters/inch. If you want the unit of velocity

to be feet/min, you can determine the conversion factor by using the following equation:

(.)

You should enter a conversion factor of ., which is equal to ./.

Chapter : Fluent Expressions Language

.. Introduction to Expressions

The Fluent Expression Language is an interpreted, declarative language based on Python, that enables

you to:

Specify complex boundary conditions and source terms with respect to time, iteration number, position,

and solution variables.

Specify various model and solver settings in terms of time or iteration.

... Expression Syntax

An expression is a string representing a combination of values, variables, operators, and function calls

that returns a value when evaluated with appropriate values for the variables.

For example: Vmax*(.*exp(-t-. [s]/. [s]))

The following sections cover the basic elements of proper expression syntax:

.... Expression Data Types

.... Expression Values

.... Expression Operations and Functions

The evaluated result of an expression can be a real number, a boolean, a real field or a boolean field.

For example, *StaticPressure evaluates to a real field when computed on a zone. Whereas,

average(*StaticPressure, ["inlet"]) evaluates to a single real values.

Note

Cell registers evaluate as boolean.

Values can be real numbers (for example, .0e-), integers (for example, -, , ), booleans (true

or false), or quantities. Quantities are real numbers with units associated. The syntax supported for

quantities is <number> [ <unit> ], for example, . [Pa kg^- s]. The unit specification

is based on CFX (Units Syntax in the CFX-Pre User's Guide).

All of the following mathematical functions take inputs in the form of an expression that evaluates

to a real number or a real field and return a real number or real field:

Table . : Operations and Functions

Function

+, -, *, /, ** (power), >, >=, <, <=, ==, !=

Operators

AND(<expr>, <expr>, …)

IF(<cond>, <true_value>, <false_value>)

NOT(<expr>)

OR(<expr>, <expr>, …)

XOR(<expr>)

acosh(<expr>)

Hyperbolic

asinh(<expr>)

atanh(<expr>)

cosh(<expr>)

sinh(<expr>)

tanh(<expr>)

abs(<expr>)

Mathematical

ceil(<expr>)

exp(<expr>)

floor(<expr>)

log(<expr>)

log10(<expr>)

max(<expr>, <expr>, …)

min(<expr>,<expr>, …)

mod(<expr>, <expr>)

round(<expr>)

sqrt(<expr>)

trunc(<expr>)

Area([<location>, <location>, …])

Reduction

Fluent Expressions Language

Function

Average(<expr>, [<location>, <location>,

…], Weight=None|"Area"|Volume")

Maximum(<expr>, [<location>, <location>,

…])

Minimum(<expr>, [<location>, <location>,

…])

Sum(<expr>, [<location>, <location>, …],

Weight=None|"Area"|Volume")

Volume([<location>, <location>, …])

acos(<expr>)

Trigonometric

asin(<expr>)

atan(<expr>)

atan2(<expr>, <expr>)

cos(<expr>)

sin(<expr>)

tan(<expr>)

Operations

Components of vectors can be accessed with the .x, .y, and the .z suffixes; magnitude can be ac-

cessed with the .mag suffix.

Important

Important

Do not use multiple comparison operators within a single expression, as the operation will

not work as intended. For example, [K]>--> StaticTemperature > [K]

will not work. To accomplish this expression, use AND(StaticTemperature>[K],

StaticTemperature<[K]).

IF Statements

The IF(<cond>, <true_value>, <false_value>) function returns the <true_value> if

<cond> is true, else it returns the <false_value>. Any of the arguments can be fields. The type

and unit dimension of <true_value> and <false_value> must be the same.

OR Statements

OR(<cond1>, <cond2>) returns true if any of the conditions (any of which can be a boolean

field) returns true.

Introduction to Expressions

AND Statements

AND(<cond1>, <cond2>) returns true if all of the conditions (any of which can be a boolean

... Units Validation

Expressions are validated to ensure they have consistent unit types. For example, Fluent flags  [cm]

+ TotalPressure because centimeters are not units of pressure. Note that units can still be provided

in different unit systems, for example,  [atm] +  [Pa].

.. Expression Sources

Expression sources are the variables that can be used in expressions.

... Field Variables

... Solution Variables

... Scientific Constants

... Aliases

A subset of the Fluent postprocessing field variables are available for use in expressions. See Appendix:

Supported Field Variables (p. ) for a listing of all the available field variables.

The following solution variables are available:

Table . : Solution Variables

Variable

Current time*

Time

In steady state, time

evaluates as , unless

the case was run in

transient, then

switched to steady

state, in which case it

will evaluate as the

latest time from the

transient run.

Current time step*

Timestep

In steady state,

timestep evaluates as

, unless the case was

run in transient, then

Variable

latest timestep from

the transient run.

Current time step size*

DeltaTime

In steady state, delta

time evaluates as ,

unless the case was run

in transient, then

latest delta time from

Global iteration count

Iteration

Table . : Scientific Constants

Value

Variable

.

Pi

PI

.

e (base of the natural logarithm)

e

. [J K^- mol^-]

Gas constant

R

.02214199e23 [mol^-]

Avogadro's number

avogadro

. [J K^-]

Boltzmann constant

boltzmann

.99792458e8 [m s^-]

Light velocity

clight

.60217653e- [A s]

Electron charge

echarge

. [m s^-]

Acceleration due to gravity

g

.62606876e- [J s]

Planck's constant

planck

.670400e- [W m^- K^-]

Stephan-Boltzmann constant

stephan

. *PI*.0e- [N A^-]

Magnetic permeability

mupermo

./(clight*clight*mupermo)

Electric constant

epspermo

Aliases provide simplified syntax to access frequently used variables.

Table . : Aliases

Alias to

Variable

Position.x

x

Position.y

y

Position.z

z

Velocity.x

u

Expression Sources

Alias to

Variable

Velocity.y

v

Velocity.z

w

Time*

t

Alias to

Variable

x

y

z

u

Alias to

Variable

v

w

Time*

t

DeltaTime*

dt

iter

StaticTemperature

T

StaticPressure

P

MassFraction

mf

.. Creating and Using Expressions

There are two ways that you can create expressions in ANSYS Fluent. The first way is by creating an

expression directly in the field where it will be applied. The second is by creating a named expression,

which can be reused at multiple locations. These two formats are discussed in the following sections:

... Directly Applied Expressions

... Named Expressions

... Context Specification

Important

Be careful to avoid situations where you are creating a circular dependency for a field or

property. For example, setting the Velocity Magnitude field of a velocity inlet to Velo-

city.mag, without specifying a value for the velocity magnitude elsewhere, results in a -

value for the velocity magnitude.

You can use expressions at boundary and cell zone conditions at fields and properties where profiles

and parameters can also be defined. Expressions can also be used at most other non-cell zone or

boundary condition locations where parameters can be defined.

To define an expression for a boundary or cell zone condition:

. Open the dialog box for the boundary/cell zone where you want to create an expression. For example, the

Velocity Inlet dialog box.

. Click the drop-down arrow to the right of the field that you would like to define using an expression and

select expression.

. You can enter your expression directly in the text field. ANSYS Fluent provides messaging regarding the

validity of the expression as soon as you begin entering it.

Alternatively, you can click

to open a bigger editor (Figure . : The Expression Editor Dialog

Box (p. )).

Creating and Using Expressions

Figure . : The Expression Editor Dialog Box

Expressions in the Console

You can specify expressions for settings through the text user interface (Console). To do so, enter a

string instead of a real value to specify a setting as an expression. For example:

You can create named expressions through the graphical user interface (GUI) via the Tree.

Setup → Named Expressions

New...

Figure . : The Expression Dialog Box

. Provide a Name for the expression. The name must start with a letter and it may contain numbers and un-

derscores.

Note

It may cause confusion if you create named expressions with names that match expression

functions such as "exp" and "abs".

. Enter the Definition of the expression. You can use the drop-downs to the right of the Definition text box

to add functions, variables, cell registers, constants, report definitions, and existing expressions to this expression

All of the supported variables are listed in the drop-down list.

Note

Note

When you use curly brackets "{}" to specify the name of a defined object, such as a report

definition or cell register, automatic suggestions are disabled and you must provide the

display name of that object.

. (Optional) Add a Description of the expression.

. (Optional) Enable Use as parameter, if you want to use the named expression as an input parameter.

Refer to Defining and Viewing Parameters (p. ) for additional information on parameters.

. Click OK to create the expression.

The Used In field lists the locations where the expression is used, including other expressions.

You can use a named expression to define other expressions—both inline expressions and named

expressions. For example, a named expression with the name Vel_magnitude can be used to setup

the velocity magnitude setting of an inlet as follows:

Note

Expressions that are in use cannot be deleted.

You can create and modify named expressions through the define/named-expressions/

text command in the console.

Important

Expressions must be dimensionally consistent. For example, you cannot add two quantities

that have different unit dimensions.

Saving and Importing Named Expressions

You have the option of saving some or all of the named expressions you create to a file for future use.

Click Export To File... to choose a directory and save your expression(s) to a file.

Click Import From File... to select and load an expression file.

Some variables require additional context before they can be evaluated. For example, MassFraction

requires the species context. Velocity may require phase context when it is evaluated in a multiphase

simulation. The context is specified as a keyword argument to a function call on the variable. For ex-

ample, MassFraction(species="co2", phase="smoke").

.. Expression Examples

The following are a few examples that demonstrate why or where you may want to use an expression

and how you would do so for these situations.

... Parabolic Inflow Profile

...Time-Varied Parabolic Inflow

... Controlled Outlet Temperature

The following example shows you how to define a parabolic inlet profile for laminar pipe flow, as

shown in Figure . : Contours of Velocity - Parabolic Inflow (p. ). In this example, the pipe is centered

in the X and Z directions and the pipe axis is aligned to the Y-direction.

Expression Examples

Figure . : Contours of Velocity - Parabolic Inflow

The expression for defining the parabolic inflow shown in Figure . : Contours of Velocity - Parabolic

Inflow (p. ) is Equation . (p. ),

(.)

Where

is the velocity at the axis,

is the radius of the pipe, and

is the local radial

coordinate.

To fully define this example:

. Create a named expression for the maximum velocity called umax.

New...

a.

Enter umax for the Name.

b. Enter . [m/s] for the Definition and click OK.

. Create an expression for the radius of the pipe.

a.

Open the Expressions dialog box by right-clicking Named Expressions in the outline view tree and

selecting New....

b. Enter Radius for the Name.

c.

a.

c.

Enter sqrt(Area(["in"])/PI) for the Definition. "in" is the name of the inlet boundary. PI is the expression

constant for Pi.

d. Click OK to create the named expression.

. Create an expression for the local radial profile.

a.

Open the Expressions dialog box and enter radius for the Name.

b. Enter sqrt(x**+z**) for the Definition. This expression uses the square root mathematical expression

operator.

c.

Click OK to create the named expression.

. Create an expression for the inlet velocity profile. This expression combines the other expressions you created.

a.

Open the Expressions dialog box and enter uprofile for the Name.

b. Enter umax*(- (radius/Radius)**) for the Definition. You can use the Expressions drop-down to the

right of the Definition box to add named expressions to your expression definition as an alternative to

typing the names manually.

c.

. Assign uprofile to the velocity inlet.

Setup → Boundary Conditions → Inlet → in

Edit...

You can group the boundary conditions by type to organize the boundaries and reduce the size of the

list. This can be accomplished by right-clicking Boundary Conditions in the tree and selecting Group

By> Zone Type.

a.

Select expression from the drop-down to the right of Velocity Magnitude.

b. Enter uprofile in the Velocity Magnitude field and click OK.

The following example shows you how to define a parabolic inlet profile for laminar pipe flow that

varies over time (a sine function with a period of  seconds). The velocity profile in this example is

the same as for Parabolic Inflow Profile (p. ) except it is for a transient simulation because the velocity

varies over time. Figure . : Parabolic Inflow Velocity Over Time (p. ) plots the area weighted average

of the velocity magnitude over  seconds.

Figure . : Parabolic Inflow Velocity Over Time

To create an expression for this time-varied velocity profile:

. Define all of the named expressions as described in Parabolic Inflow Profile (p. ).

. Create an expression for omega.

New...

a.

Enter omega for the Name.

b. Enter *PI / ([s]) for the Definition and click OK.

. Create an expression for the velocity profile that varies over time.

a.

Open the Expressions dialog box and enter uprofile_transient for the Name.

b. Enter uprofile*(sin(omega*Time)*. + ) for the Definition and click OK.

. Assign uprofile_transient to the velocity inlet.

Edit...

a.

b. Enter uprofile_transient in the Velocity Magnitude field and click OK.

The following example shows you how to drive the maximum temperature at the outlet to a target

temperature by varying the inlet temperature. For this scenario, a pipe with laminar flow has a part

of the wall that is heated to  Kelvin and a target outlet temperature of  Kelvin (Figure . : Pipe

Geometry Colored by ID (Heated Wall is Green) (p. ) shows the portion of the wall that is heated).

A controller turns on every 10th iteration (steady-state case) and adjusts the inlet temperature according

to Equation . (p. ). In the other iterations, the controller leaves the temperature unchanged. This

is achieved by using the conditional statement given in Equation . (p. ). Figure . : Contours of

Temperature (outlet is closest) (p. ) shows the developed temperature profile for this case.

(.)

(.)

is the formula used to adjust the inlet temperature,

is the current inlet temperature,

is the target temperature for the outlet, which is set to  Kelvin,

is the maximum

temperature at the outlet, and

is a relaxation factor.

Figure . : Pipe Geometry Colored by ID (Heated Wall is Green)

Figure . : Contours of Temperature (outlet is closest)

Figure . : Plots of Inlet Temperature, Average Outlet Temperature, and Maximum Outlet

The following steps show how to create the expressions used in this example:

. Create a named expression for the initial temperature, called TStart.

New...

a.

Enter TStart for the Name.

b. Enter  [K] for the Definition and click OK.

. Create an expression for the target temperature for the outlet, called TTarget, and set it equal to  [K].

Use the same process that you used to create TStart.

. Create an expression for the maximum temperature that occurs at the outlet, called TMaxOut. In this ex-

pression you will be using a function to determine the maximum temperature.

a.

Click the Functions drop-down and select Reduction → Maximum.

b. Enter StaticTemperature for the first field of the function and ["out"] for the location.The total ex-

pression should appear as Maximum(StaticTemperature, ["out"]).

. Create an expression for the current inlet temperature, called TInCurrent, and set it equal to Average(Stat-

icTemperature, ["in"],Weight=None). Use a similar process to what you used to create TMaxOut, but with

selecting the Average function instead.

. Create an expression for the relaxation factor, called relax, and set it equal to ..

. Create an expression for adjusting the inlet temperature, called TAdjust, and set it equal to TInCurrent

+ (TTarget - TMaxOut)*relax.

. Create an expression for the inlet temperature, which will be called TIn, and set it equal to IF(iter<,

TStart, IF(mod(iter+, )==,TAdjust,TInCurrent)). Use a similar process to what you used to create

TMaxOut, but with selecting the IF  conditional function instead.

. Assign TIn to the inlet.

Edit...

a.

Select expression from the drop-down to the right of Temperature.

b. Enter TIn in the Temperature field and click OK.

.. Appendix: Supported Field Variables

Table . : Field Variables

Variable (type)

AbsolutePressure (scalar)

Absolute Pressure

AbsoluteIRSolarFlux (scalar)

Absolute IR Solar Flux

AbsoluteRadiationFlux (scalar)

Absolute Radiation Flux

AbsoluteVisibleSolarFlux (scalar)

Absolute Visible Solar Flux

AbsorptionCoefficient (scalar)

Absorption Coefficient

Accumulated Deformation (scalar)

Accumulated Deformation

Appendix: Supported Field Variables

AcentricFactor (scalar)

Acentric Factor

AcousticPower (scalar)

Acoustic Power

AcousticPowerLeveldB (scalar)

Acoustic Power Level (dB)

ActiveElementPartition (scalar)

Active Cell Partition

AdaptionCurvature (scalar)

Adaption Curvature

AdaptionFunction (scalar)

Adaption Function

AdaptionIsoValue (scalar)

Adaption Iso-Value

AdaptionSpaceGradient (scalar)

Adaption Space Gradient

AdaptionFlameTemperature (scalar)

Adaption Flame Temperature

AdjointAp (scalar)

Adjoint Ap

AdjointLocalSolutionMaker (scalar)

Adjoint Local Solution Maker

ArtificialDissipation (scalar)

Artificial Dissipation

ArtificialInterfacialViscosity (scalar)

Artificial Interfacial Viscosity

AxialVelocity (scalar)

Axial Velocity

BCDNormalizedVariableU (scalar)

BCD Normalized Variable U

BCDNormalizedVariableV (scalar)

BCD Normalized Variable V

BCDNormalizedVariableW (scalar)

BCD Normalized Variable W

BackgroundSizingFunction (scalar)

Background Sizing Function

BeamIrradiationFlux (scalar)

Beam Irradiation Flux

BlendingFunctionforGEKO (scalar)

Blending Function for GEKO

BodyForceMagnitude (scalar)

Body Force Magnitude

BodyForced (vector)

Body-Force-d%s

BoundaryCellDistance (scalar)

Boundary Cell Distance

BoundaryVolumeDistance (scalar)

Boundary Volume Distance

CapillaryPressure (scalar)

Capillary-Pressure

CellAR (scalar)

Cell AR

CellARDirectional (scalar)

Cell AR Directional

CellARRatio (scalar)

Cell AR Ratio

CellARRatioTag (scalar)

Cell AR Ratio Tag

CellBoundaryDistanceMeshSmoothing (scalar)

Cell Boundary Distance Mesh

Smoothing

CellBoundaryDistanceOverset (scalar)

Cell Boundary Distance Overset

CellCFLMultiplier (scalar)

Cell CFL Multiplier

CellChildren (scalar)

Cell Children

CellElementType (scalar)

Cell Element Type

CellEquiangleSkew (scalar)

Cell Equiangle Skew

CellEquivolumeSkew (scalar)

Cell Equivolume Skew

CellID (scalar)

Cell ID

CellIndex (scalar)

Cell Index

CellMachine (scalar)

Cell Machine

CellMap (scalar)

Cell Map

CellMind (scalar)

Cell Min d

CellMindDirectional (scalar)

Cell Min d Directional

CellMindRatio (scalar)

Cell Min d Ratio

CellNormalizedSumFaceArea (scalar)

Cell Normalized Sum Face Area

CellRefineLevel (scalar)

Cell Refine Level

CellSquishIndex (scalar)

Cell Squish Index

CellSurfaceArea (scalar)

Cell Surface Area

CellTimeScale (scalar)

Cell Time Scale

CellVolume (scalar)

Cell Volume

CellVolumeChange (scalar)

Cell Volume Change

CellVolumeDerivative (scalar)

Cell Volume Derivative

CellVolumeError (scalar)

Cell Volume Error

CellWarpage (scalar)

Cell Warpage

CellWeight (scalar)

Cell Weight

CellZoneCounter (scalar)

Cell Zone Counter

CellZoneIndex (scalar)

Cell Zone Index

CellZoneType (scalar)

ChemicalTimeScale (scalar)

Chemical Time Scale

CompressibilityFactor (scalar)

Compressibility Factor

ConnectedRegion (scalar)

Connected Region

ConservedMassFraction (scalar with species)

Conserved Mass Fraction of %s

ContactCellMark (scalar)

Contact Cell Mark

ContactResistivity (scalar)

Contact Resistivity

ConvectionTimeStep (scalar)

Convection Time Step

CriticalPressure (scalar)

Critical Pressure

CriticalSpecificVolume (scalar)

Critical Specific Volume

CriticalStrainRate (scalar)

Critical Strain Rate

CriticalTemperature (scalar)

Critical Temperature

CurvatureCorrectionFunctionfr (scalar)

Curvature Correction Function fr

DESLengthScale (scalar)

DES Length Scale

DESTKEDissipationMultiplier (scalar)

DES TKE Dissipation Multiplier

DPMAbsorptionCoefficient (scalar)

DPM Absorption Coefficient

DPMAccretion (scalar)

DPM Accretion

DPMAccretionRate (scalar)

DPM Accretion Rate

DPMApproachingPackingLimit (scalar)

DPM Approaching Packing Limit

DPMBurnout (scalar)

DPM Burnout

DPMCollisionRate (scalar)

DPM Collision Rate

DPMConcentration (scalar)

DPM Concentration

DPMDomainPartition (scalar)

DPM Domain Partition

DPMEmission (scalar)

DPM Emission

DPMEnthalpySource (scalar)

DPM Enthalpy Source

DPMEvaporationDevolatilization (scalar)

DPM Evaporation/Devolatilization

DPMMassSource (scalar)

DPM Mass Source

DPMMomentumSource (vector)

DPM %s Momentum Source

DPMNumberDensity (scalar)

DPM Number Density

DPMNumberofParcels (scalar)

DPM Number of Parcels

DPMNumberofParticles (scalar)

DPM Number of Particles

DPMScattering (scalar)

DPM Scattering

DPMSensibleEnthalpySource (scalar)

DPM Sensible Enthalpy Source

DPMSource (scalar with species)

DPM %s Source

DPMSpecificTurbulentDissipationSource (scalar)

DPM Specific Turbulent Dissipation

Source

DPMStepsperCell (scalar)

DPM Steps per Cell

DPMTurbulentDissipationSource (scalar)

DPM Turbulent Dissipation Source

DPMTurbulentKineticEnergySource (scalar)

DPM Turbulent Kinetic Energy

Source

DPMUUReynoldsStressSource (scalar)

DPM UU Reynolds Stress Source

DPMUVReynoldsStressSource (scalar)

DPM UV Reynolds Stress Source

DPMUWReynoldsStressSource (scalar)

DPM UW Reynolds Stress Source

DPMVVReynoldsStressSource (scalar)

DPM VV Reynolds Stress Source

DPMVWReynoldsStressSource (scalar)

DPM VW Reynolds Stress Source

DPMVelocityMagnitude (scalar)

DPM Velocity Magnitude

DPMVolume (scalar)

DPM Volume

DPMVolumeFraction (scalar)

DPM Volume Fraction

DPMWWReynoldsStressSource (scalar)

DPM WW Reynolds Stress Source

DPMWallForce (vector)

DPM Wall %s Force

DPMWallNormalPressure (scalar)

DPM Wall Normal Pressure

DQMOM-m4 (scalar)

DQMOM-m4

DRGReducedNumberofReactions (scalar)

DRG Reduced Number of Reactions

DRGReducedNumberofSpecies (scalar)

DRG Reduced Number of Species

DamkohlerNumber (scalar)

Damkohler Number

Density (scalar)

Density

DensityAll (scalar)

Density All

Diameter (scalar)

Diameter

DiffusionTimeStep (scalar)

Diffusion Time Step

DiffusivityMeshSmoothing (scalar)

Diffusivity mesh Smoothing

DropletAverageRadiusmicrons (scalar)

Droplet Average Radius (microns)

DropletCriticalRadiusmicrons (scalar)

Droplet Critical Radius (microns)

DropletGrowthRatemicronss (scalar)

Droplet Growth Rate (microns/s)

DropletSurfaceTension (scalar)

Droplet Surface Tension

DynamicAlgebraicVarianceConstant (scalar)

Dynamic Algebraic Variance

Constant

DynamicCellVolumeChange (scalar)

Dynamic Cell Volume Change

DynamicPressure (scalar)

Dynamic Pressure

DynamicPrismFaceCavMarks (scalar)

Dynamic Prism Face Cav. Marks

DynamicViscosity (scalar)

Molecular Viscosity

EDCCellVolumeFraction (scalar)

EDC Cell Volume Fraction

EdgeLengthRatio (scalar)

Edge Length Ratio

EffDiffCoefof (scalar with species)

Eff Diff Coef of %s

EffectivePrandtlNumber (scalar)

Effective Prandtl Number

EffectiveThermalConductivity (scalar)

Effective Thermal Conductivity

EffectiveViscosity (scalar)

Effective Viscosity

ElectricCurrentMagnitude (scalar)

Electric Current Magnitude

ElectricPotential (scalar)

Electric Potential

ElectricalConductivity (scalar)

Electrical Conductivity

ElectrodeSurfacePotential (scalar)

Electrode Surface Potential

ElementAcousticCourantNumber (scalar)

Cell Acoustic Courant Number

ElementAspectRatio (scalar)

ElementConvectionCourantNumber (scalar)

Cell Convective Courant Number

ElementReynoldsNumber (scalar)

Cell Reynolds Number

ElementWallDistance (scalar)

Cell Wall Distance

EllipticRelaxationFunction (scalar)

Elliptic Relaxation Function

EnthalpyAp (scalar)

Enthalpy Ap

EnthalpySource (scalar)

Enthalpy Source

Enthalpyof (scalar with species)

Enthalpy of %s

Entropyof (scalar with species)

Entropy of %s

EquilibriumMassfractionof (scalar with species)

Equilibrium Mass fraction of %s

EquilibriumTemperature (scalar)

Equilibrium Temperature

EvaporationHeatFlux (scalar)

Evaporation Heat Flux

ExistingValue (scalar)

Existing Value

ExpansionRatio (scalar)

Expansion Ratio

ExternalTemperatureShell (scalar)

External Temperature (Shell)

F1DampingFunction (scalar)

F- Damping Function

F2DampingFunction (scalar)

FaceAreaMagnitude (scalar)

Face Area Magnitude

FaceHandedness (scalar)

FaceRadiation (scalar)

Face Radiation

FaceSkew (scalar)

Face Skew

FaceSquishIndex (scalar)

Face Squish Index

FaceWarpage (scalar)

Face Warpage

FaradaicCurrentDensity (scalar)

Faradaic Current Density

FaradaicHeatSource (scalar)

Faradaic Heat Source

FaradaicVoltageJump (scalar)

Faradaic Voltage Jump

FaradaicVoltageResistance (scalar)

Faradaic Voltage Resistance

FilmCourantNumber (scalar)

Film Courant Number

FilmCoverage (scalar)

Film Coverage

FilmDPMEnergySource (scalar)

Film DPM Energy Source

FilmDPMMassSource (scalar)

Film DPM Mass Source

FilmDPMXMomentumSource (scalar)

Film DPM X-Momentum Source

FilmDPMYMomentumSource (scalar)

Film DPM Y-Momentum Source

FilmDPMZMomentumSource (scalar)

Film DPM Z-Momentum Source

FilmDensity (scalar)

Film Density

FilmEffectivePressure (scalar)

Film Effective Pressure

FilmMass (scalar)

Film Mass

FilmOutflowMass (scalar)

Film Outflow Mass

FilmPassiveScalar (scalar)

Film Passive Scalar

FilmPhaseChangeRate (scalar)

Film Phase Change Rate

Film Mass

FilmSecondaryPhaseCollectionCoef (scalar)

Film Secondary Phase Collection

Coef

FilmSecondaryPhaseMass (scalar)

Film Secondary Phase Mass

FilmSeparatedDiam (scalar)

Film Separated Diam

FilmSeparatedMass (scalar)

Film Separated Mass

FilmSeparationRate (scalar)

Film Separation Rate

FilmStrippedDiam (scalar)

Film Stripped Diam

FilmStrippedMass (scalar)

Film Stripped Mass

FilmStrippingRate (scalar)

Film Stripping Rate

FilmStrippingWeberNumber (scalar)

Film Stripping Weber Number

FilmSurfaceTemperature (scalar)

Film Surface Temperature

FilmSurfaceVelocity (vector)

Film Surface %s-Velocity

FilmSurfaceVelocityMagnitude (scalar)

Film Surface Velocity Magnitude

FilmTemperature (scalar)

Film Temperature

FilmThickness (scalar)

Film Thickness

FilmVelocity (vector)

Film %s-Velocity

FilmVelocityMagnitude (scalar)

Film Velocity Magnitude

FilmWeberNumber (scalar)

Film Weber Number

FineScaleMassfractionof (scalar with species)

Fine Scale Mass fraction of %s

FineScaleTemperature (scalar)

Fine Scale Temperature

FiniteRateSource (scalar)

Finite-Rate Source

FlameAreaDensity (scalar)

Flame Area Density

FlameAreaDestruction (scalar)

Flame Area Destruction

FlameAreaProductionP1 (scalar)

Flame Area Production P1

FlameAreaProductionP2 (scalar)

Flame Area Production P2

FlameAreaProductionP3 (scalar)

Flame Area Production P3

FlameAreaProductionP4 (scalar)

Flame Area Production P4

FlameletMeanTemperature (scalar)

Mean Temperature

Fmean2Ap (scalar)

Fmean2 Ap

Fmean2Source (scalar)

Fmean2 Source

Fmean2 Ap

FmeanAp (scalar)

Fmean Ap

FmeanSource (scalar)

Fmean Source

FmuDampingFunction (scalar)

F-mu Damping Function

FrictionalViscosity (scalar)

Frictional Viscosity

Fvar2Ap (scalar)

Fvar2 Ap

Fvar2Prod (scalar)

Fvar2 Prod

Fvar2Source (scalar)

Fvar2 Source

FvarAp (scalar)

Fvar Ap

FvarProd (scalar)

Fvar Prod

FvarSource (scalar)

Fvar Source

GasConstantR (scalar)

Gas Constant (R)

GeometricRoughnessHeight (scalar)

Geometric Roughness Height

GequationAp (scalar)

G-equation Ap

GequationSource (scalar)

G-equation Source

GradientQualityMeasure (scalar)

Gradient Quality Measure

GranularBulkViscosity (scalar)

Granular Bulk Viscosity

GranularConductivity (scalar)

Granular Conductivity

GranularPressure (scalar)

Granular Pressure

GranularPressureGcmpn (vector)

Granular Pressure G %s cmpn

GranularTemperature (scalar)

Granular Temperature

GvarianceAp (scalar)

G-variance Ap

GvarianceSource (scalar)

G-variance Source

HTCCellMark (scalar)

HTC Cell Mark

HTCLBBoundaryZones (scalar)

HTC LB Boundary Zones

HTCLBVolumeFraction (scalar)

HTC LB Volume Fraction

HeatExchangerSource (scalar)

Heat Exchanger Source

HeatReleaseRate (scalar)

Heat Release Rate

HeatTransferCoefficient (scalar)

Surface Heat Transfer Coef.

HeatofHeterogeneousReaction (scalar)

Heat of Heterogeneous Reaction

HeatofReaction (scalar)

Heat of Reaction

Helicity (scalar)

Helicity

HreconNorm (scalar)

Hrecon Norm

HviscNorm (scalar)

Hvisc Norm

IgnitionVariable (scalar)

Ignition Variable

IgnitionVariableProduction (scalar)

Helicity

Hvisc Norm

Ignition Variable Production

IncidentRadiation (scalar)

Incident Radiation

IncidentRadiationInner (scalar)

Incident Radiation (Inner)

InertDensity (scalar)

Inert Density

InertEnthalpy (scalar)

Inert Enthalpy

InertMassFraction (scalar)

Inert Mass Fraction

InertSpecificHeat (scalar)

Inert Specific Heat

InertialConvectiveVariance (scalar)

Inertial-Convective Variance

InterfaceOverlapFraction (scalar)

Interface Overlap Fraction

InterfaceWallIDs (scalar)

Interface Wall IDs

InterfacialAreaConcentration (scalar)

Interfacial Area Concentration

IntermittencyAp (scalar)

Intermittency Ap

IntermittencyEffective (scalar)

Intermittency Effective

IntermittencyEffectiveSmooth (scalar)

Intermittency Effective Smooth

IntermittencySource (scalar)

Intermittency Source

IntermittentTurbNetFlameStretch (scalar)

Intermittent Turb Net Flame Stretch

JetAcousticPower (scalar)

Jet Acoustic Power

JetAcousticPowerLeveldB (scalar)

Jet Acoustic Power Level (dB)

JouleHeatSource (scalar)

Joule Heat Source

LEESelfNoiseXSource (scalar)

LEE Self-Noise X-Source

LEESelfNoiseYSource (scalar)

LEE Self-Noise Y-Source

LEESelfNoiseZSource (scalar)

LEE Self-Noise Z-Source

LEEShearNoiseXSource (scalar)

LEE Shear-Noise X-Source

LEEShearNoiseYSource (scalar)

LEE Shear-Noise Y-Source

LEEShearNoiseZSource (scalar)

LEE Shear-Noise Z-Source

LEETotalNoiseXSource (scalar)

LEE Total Noise X-Source

LEETotalNoiseYSource (scalar)

LEE Total Noise Y-Source

LEETotalNoiseZSource (scalar)

LEE Total Noise Z-Source

LESSubgridTurbulentViscosity (scalar)

LES Subgrid Turbulent Viscosity

LamDiffCoefof (scalar with species)

Lam Diff Coef of %s

Lambda2Criterion (scalar)

Lambda  Criterion

LaminarFlameSpeed (scalar)

Laminar Flame Speed

LaminarFlameThickness (scalar)

Laminar Flame Thickness

LaminarKineticEnergy (scalar)

Laminar Kinetic Energy

LevelsetFunction (scalar)

Level-set Function

LilleysSelfNoiseSource (scalar)

Lilley's Self-Noise Source

LilleysShearNoiseSource (scalar)

Lilley's Shear-Noise Source

LilleysTotalNoiseSource (scalar)

Lilley's Total Noise Source

LiquidDensityLiquidPhase (scalar)

Liquid Density (Liquid-Phase)

LiquidFraction (scalar)

Liquid Fraction

LiquidMassFraction (scalar)

Liquid Mass Fraction

LiquidMassGenerationRate (scalar)

Liquid Mass Generation Rate

LiquidPhaseHeatFlux (scalar)

Liquid Phase Heat Flux

LiquidSpeciesMassFraction (scalar with species)

Liquid species mass fraction of %s

LiquidusTemperature (scalar)

Liquidus Temperature

LocalIgnitionTime (scalar)

Local Ignition Time

Log10DropletsNucleationRate (scalar)

Log10(Droplets Nucleation Rate)

Log10DropletsPerUnitVolume (scalar)

Log10(Droplets Per Unit Volume)

LumpID (scalar)

Lump ID

MPPSource (scalar)

MP P Source

MachNumber (scalar)

Mach Number

MagnitudeofSensitivitytoBodyForces (scalar)

Magnitude of Sensitivity to Body

Forces

MagnitudeofSensitivitytoBodyForcesCellValues

(scalar)

Forces (Cell Values)

MarkPoorElements (scalar)

Mark Poor Elements

MassFraction (scalar with species)

Mass fraction of %s

MassImbalance (scalar)

Mass Imbalance

MaxPackingLimit (scalar)

Max. Packing Limit

MeanDeformation (scalar)

Mean Deformation

MeanDistancefromFlame (scalar)

Mean Distance from Flame

MeanGranularTemperature (scalar)

Mean Granular Temperature

MeanMassFractionof (scalar with species)

Mean Mass Fraction of %s

MeanMassfraction (scalar with species)

Mean %s Mass fraction

MeanMixtureFraction (scalar)

Mean Mixture Fraction

MeanPhaseDiameter (scalar)

Mean Phase Diameter

MeanPressureCoefficient (scalar)

Mean Pressure Coefficient

MeanReactionProgress (scalar)

Mean Reaction Progress

MeanSkinFrictionCoefficient (scalar)

Mean Skin Friction Coefficient

MeanSoundPressure (scalar)

Mean Sound Pressure

MeanSoundWaveEqModelSource (scalar)

Mean Sound WaveEq Model Source

MeanStaticPressure (scalar)

Mean Static Pressure

MeanStaticTemperature (scalar)

Mean Static Temperature

MeanSurfaceHeatFlux (scalar)

Mean Surface Heat Flux

MeanSurfaceHeatTransferCoef (scalar)

Mean Surface Heat Transfer Coef.

MeanSurfaceNusseltNumber (scalar)

Mean Surface Nusselt Number

MeanSurfaceStantonNumber (scalar)

Mean Surface Stanton Number

MeanVelocityMagnitude (scalar)

Mean Velocity Magnitude

MeanVolumefraction (scalar)

Mean Volume fraction

MeanofMixtureFraction (scalar)

Mean of Mixture Fraction

MeshVariationEffect (scalar)

Mesh Variation Effect

MeshVelocity (vector)

Mesh %s-Velocity

MigrationDiffCoefof (scalar with species)

Migration Diff Coef of %s

MixtureDensity (scalar)

Mixture Density

MixtureFractionVariance (scalar)

Mixture Fraction Variance

ModifiedTurbViscosityAp (scalar)

Modified Turb Viscosity Ap

ModifiedTurbViscositySource (scalar)

Modified Turb Viscosity Source

ModifiedTurbulenceViscosity (scalar)

Modified Turbulent Viscosity

MolarConcentration (scalar with species)

Molar Concentration of %s

MoleFraction (scalar with species)

Mole fraction of %s

MolecularMass (scalar)

Mean Molecular Weight

MomThicknReAp (scalar)

Mom. Thickn. Re Ap

MomThicknReSource (scalar)

Mom. Thickn. Re Source

MomentumThicknessRe (scalar)

Momentum Thickness Re

NetFlameAreaProduction (scalar)

Net Flame Area Production

NetReactionRateof (scalar with species)

Net Reaction Rate of %s

NodePairCheck (scalar)

Node Pair Check

NonEquilibriumThermalModelSource (scalar)

Non-Equilibrium Thermal Model

Source

Normalizedvolumefraction (scalar)

Normalized volume fraction

NormalOptimalDisplacement (scalar)

Normal Optimal Displacement

NormalShapeSensitivity (scalar)

Normal Shape Sensitivity

NormalizedQCriterion (scalar)

Normalized Q Criterion

OrthogonalQuality (scalar)

Orthogonal Quality

OversetCellType (scalar)

Overset Cell Type

OversetDonorCount (scalar)

Overset Donor Count

OversetReceptorCount (scalar)

Overset Receptor Count

PDFDepartureEnthalpy (scalar)

PDF Departure Enthalpy

PDFLaminarFlameSpeed (scalar)

PDFMeanTemperature (scalar)

PDFStaticTemperature (scalar)

Static Temperature

PDFTableAdiabaticEnthalpy (scalar)

PDF Table Adiabatic Enthalpy

PDFTableHeatLossGain (scalar)

PDF Table Heat Loss/Gain

PHI (scalar)

PHI

ParticleTimeStep (scalar)

Particle Time Step

PartitionNeighbors (scalar)

Partition Neighbors

PdfEnthalpy (scalar)

Pdf Enthalpy

PdfFmean (scalar)

Pdf Fmean

PdfFvar (scalar)

Pdf Fvar

PhaseID (scalar)

Phase ID

PollutantCorrectionAp (scalar)

Pollutant Correction Ap

PollutantCorrectionSource (scalar)

Pollutant Correction Source

Position (vector)

%s-Coordinate

PrandtlNumber (scalar)

Molecular Prandtl Number

PreconditioningReferenceVelocity (scalar)

Preconditioning Reference Velocity

PressureCoefficient (scalar)

Pressure Coefficient

PressureCorrectionAp (scalar)

Pressure Correction Ap

PressureCorrectionSource (scalar)

Pressure Correction Source

PressureSpectrumIm0 (scalar)

Pressure Spectrum Im

PressureSpectrumIm1 (scalar)

PressureSpectrumIm10 (scalar)

PressureSpectrumIm11 (scalar)

PressureSpectrumIm12 (scalar)

PressureSpectrumIm13 (scalar)

PressureSpectrumIm14 (scalar)

PressureSpectrumIm15 (scalar)

PressureSpectrumIm16 (scalar)

PressureSpectrumIm17 (scalar)

PressureSpectrumIm18 (scalar)

PressureSpectrumIm19 (scalar)

PressureSpectrumIm2 (scalar)

PressureSpectrumIm3 (scalar)

PressureSpectrumIm4 (scalar)

PressureSpectrumIm5 (scalar)

PressureSpectrumIm6 (scalar)

PressureSpectrumIm7 (scalar)

PressureSpectrumIm8 (scalar)

PressureSpectrumIm9 (scalar)

PressureSpectrumRe0 (scalar)

Pressure Spectrum Re

PressureSpectrumRe1 (scalar)

PressureSpectrumRe10 (scalar)

PressureSpectrumRe11 (scalar)

PressureSpectrumRe12 (scalar)

PressureSpectrumRe13 (scalar)

PressureSpectrumRe14 (scalar)

PressureSpectrumRe15 (scalar)

PressureSpectrumRe16 (scalar)

PressureSpectrumRe17 (scalar)

PressureSpectrumRe18 (scalar)

PressureSpectrumRe19 (scalar)

PressureSpectrumRe2 (scalar)

PressureSpectrumRe3 (scalar)

PressureSpectrumRe4 (scalar)

PressureSpectrumRe5 (scalar)

PressureSpectrumRe6 (scalar)

PressureSpectrumRe7 (scalar)

PressureSpectrumRe8 (scalar)

PressureSpectrumRe9 (scalar)

ProductFormationRate (scalar)

Product Formation Rate

ProductionofEntropy (scalar)

Production of Entropy

Productionofk (scalar)

Production of k

Productionoflaminark (scalar)

Production of laminar k

ProgressVariable (scalar)

Progress Variable

ProgressVariableAp (scalar)

Progress Variable Ap

ProgressVariableGradientMagnitude (scalar)

Progress Variable Gradient

Magnitude

ProgressVariableSource (scalar)

Progress Variable Source

ProgressVariableVariance (scalar)

Progress Variable Variance

Q (scalar)

Q

QCriterion (scalar)

Q Criterion

QTimeAverage (scalar)

Q Time-Average

QuenchingHeatFlux (scalar)

Quenching Heat Flux

RMSEGranularTemperature (scalar)

RMSE Granular Temperature

RMSEMassFractionof (scalar with species)

RMSE Mass Fraction of %s

RMSEPhaseDiameter (scalar)

RMSE Phase Diameter

RMSEReactionProgress (scalar)

RMSE Reaction Progress

RMSESoundPressure (scalar)

RMSE Sound Pressure

RMSESoundWaveEqModelSource (scalar)

RMSE Sound WaveEq Model Source

RMSEStaticPressure (scalar)

RMSE Static Pressure

RMSEStaticTemperature (scalar)

RMSE Static Temperature

RMSEVelocityMagnitude (scalar)

RMSE Velocity Magnitude

RMSEVolumefraction (scalar)

RMSE Volume fraction

RMSEofMixtureFraction (scalar)

RMSE of Mixture Fraction

RMSMassfraction (scalar with species)

RMS %s Mass fraction

RMSStaticTemperature (scalar)

RMS Static Temperature

RMSTemperature (scalar)

RMS Temperature

RadialVelocity (scalar)

Radial Velocity

RadiationIntensityNormalizedStdDeviation

(scalar)

Radiation Intensity.Normalized Std

Deviation

RadiationTemperature (scalar)

Radiation Temperature

RadiativeHeatFlux (scalar)

Radiation Heat Flux

ReactorNetTemperature (scalar)

Reactor Net Temperature

ReactorNetZoneID (scalar)

Reactor Net Zone ID

ReconstructiondHd (vector)

Reconstruction dH/d%s

ReconstructiondTd (vector)

Reconstruction dT/d%s

ReconstructiondXVelocityd (vector)

Reconstruction dX-Velocity/d%s

ReconstructiondYVelocityd (vector)

Reconstruction dY-Velocity/d%s

ReconstructiondZVelocityd (vector)

Reconstruction dZ-Velocity/d%s

Reconstructionded (vector)

Reconstruction de/d%s

Reconstructiondkd (vector)

Reconstruction dk/d%s

Reconstructiondnutd (vector)

Reconstruction dnut/d%s

Reconstructiondpd (vector)

Reconstruction dp/d%s

Reconstructiondrhod (vector)

Reconstruction drho/d%s

Reconstructiondvofd (vector)

Reconstruction dvof/d%s

ReducedPressure (scalar)

Reduced Pressure

ReducedTemperature (scalar)

Reduced Temperature

ReflectedIRSolarFlux (scalar)

Reflected IR Solar Flux

ReflectedRadiationFlux (scalar)

Reflected Radiation Flux

ReflectedVisibleSolarFlux (scalar)

Reflected Visible Solar Flux

RefractiveIndex (scalar)

Refractive Index

RelativeHumidity (scalar)

Relative Humidity

RelativeStrain (scalar)

Relative Strain

RichFlammabilityFactor (scalar)

Rich Flammability Factor

RngStrainrateTerm (scalar)

Rng Strainrate Term

SASTermStrainRateMagnitude (scalar)

SAS Term Strain Rate Magnitude

SPLfor13OctaveBandat05HzdB (scalar)

SPL for /-Octave Band at .5Hz

(dB)

SPLfor13OctaveBandat063HzdB (scalar)

SPL for /-Octave Band at .63Hz

(dB)

SPLfor13OctaveBandat08HzdB (scalar)

SPL for /-Octave Band at .8Hz

(dB)

SPLfor13OctaveBandat100HzdB (scalar)

SPL for /-Octave Band at 100Hz

(dB)

SPLfor13OctaveBandat100kHzdB (scalar)

SPL for /-Octave Band at 100kHz

(dB)

(dB)

(dB)

(dB)

SPLfor13OctaveBandat10HzdB (scalar)

SPL for /-Octave Band at 10Hz

(dB)

SPLfor13OctaveBandat10kHzdB (scalar)

SPL for /-Octave Band at 10kHz

(dB)

SPLfor13OctaveBandat125HzdB (scalar)

SPL for /-Octave Band at .25Hz

(dB)

SPLfor13OctaveBandat125kHzdB (scalar)

SPL for /-Octave Band at .25kHz

(dB)

SPLfor13OctaveBandat160HzdB (scalar)

SPL for /-Octave Band at 160Hz

(dB)

SPLfor13OctaveBandat16HzdB (scalar)

SPL for /-Octave Band at .6Hz

(dB)

SPLfor13OctaveBandat16kHzdB (scalar)

SPL for /-Octave Band at .6kHz

(dB)

SPLfor13OctaveBandat1HzdB (scalar)

SPL for /-Octave Band at 1Hz (dB)

SPLfor13OctaveBandat1kHzdB (scalar)

SPL for /-Octave Band at 1kHz

(dB)

SPLfor13OctaveBandat200HzdB (scalar)

SPL for /-Octave Band at 200Hz

(dB)

SPLfor13OctaveBandat20HzdB (scalar)

SPL for /-Octave Band at 20Hz

(dB)

SPLfor13OctaveBandat20kHzdB (scalar)

SPL for /-Octave Band at 20kHz

(dB)

SPLfor13OctaveBandat250HzdB (scalar)

SPL for /-Octave Band at 250Hz

(dB)

SPLfor13OctaveBandat25HzdB (scalar)

(dB)

SPLfor13OctaveBandat25kHzdB (scalar)

SPL for /-Octave Band at .5kHz

(dB)

SPLfor13OctaveBandat2HzdB (scalar)

SPL for /-Octave Band at 2Hz (dB)

SPLfor13OctaveBandat2kHzdB (scalar)

SPL for /-Octave Band at 2kHz

(dB)

SPLfor13OctaveBandat315HzdB (scalar)

SPL for /-Octave Band at .15Hz

(dB)

SPLfor13OctaveBandat315kHzdB (scalar)

SPL for /-Octave Band at .15kHz

(dB)

SPLfor13OctaveBandat400HzdB (scalar)

SPL for /-Octave Band at 400Hz

(dB)

SPLfor13OctaveBandat40HzdB (scalar)

(dB)

(dB)

(dB)

SPL for /-Octave Band at 40Hz

(dB)

SPLfor13OctaveBandat40kHzdB (scalar)

SPL for /-Octave Band at 40kHz

(dB)

SPLfor13OctaveBandat4HzdB (scalar)

SPL for /-Octave Band at 4Hz (dB)

SPLfor13OctaveBandat4kHzdB (scalar)

SPL for /-Octave Band at 4kHz

(dB)

SPLfor13OctaveBandat500HzdB (scalar)

SPL for /-Octave Band at 500Hz

(dB)

SPLfor13OctaveBandat50HzdB (scalar)

SPL for /-Octave Band at 50Hz

(dB)

SPLfor13OctaveBandat50kHzdB (scalar)

SPL for /-Octave Band at 50kHz

(dB)

SPLfor13OctaveBandat5HzdB (scalar)

SPL for /-Octave Band at 5Hz (dB)

SPLfor13OctaveBandat5kHzdB (scalar)

SPL for /-Octave Band at 5kHz

(dB)

SPLfor13OctaveBandat630HzdB (scalar)

SPL for /-Octave Band at 630Hz

(dB)

SPLfor13OctaveBandat63HzdB (scalar)

SPL for /-Octave Band at .3Hz

(dB)

SPLfor13OctaveBandat63kHzdB (scalar)

SPL for /-Octave Band at .3kHz

(dB)

SPLfor13OctaveBandat800HzdB (scalar)

SPL for /-Octave Band at 800Hz

(dB)

SPLfor13OctaveBandat80HzdB (scalar)

SPL for /-Octave Band at 80Hz

(dB)

SPLfor13OctaveBandat80kHzdB (scalar)

SPL for /-Octave Band at 80kHz

(dB)

SPLfor13OctaveBandat8HzdB (scalar)

SPL for /-Octave Band at 8Hz (dB)

SPLfor13OctaveBandat8kHzdB (scalar)

SPL for /-Octave Band at 8kHz

(dB)

SPLforConstWidthBand0dB (scalar)

SPL for Const Width Band  (dB)

SPLforConstWidthBand10dB (scalar)

SPLforConstWidthBand11dB (scalar)

SPLforConstWidthBand12dB (scalar)

SPLforConstWidthBand13dB (scalar)

SPLforConstWidthBand14dB (scalar)

SPLforConstWidthBand15dB (scalar)

SPLforConstWidthBand16dB (scalar)

SPLforConstWidthBand17dB (scalar)

SPLforConstWidthBand18dB (scalar)

SPLforConstWidthBand19dB (scalar)

SPLforConstWidthBand1dB (scalar)

SPLforConstWidthBand2dB (scalar)

SPLforConstWidthBand3dB (scalar)

SPLforConstWidthBand4dB (scalar)

SPLforConstWidthBand5dB (scalar)

SPLforConstWidthBand6dB (scalar)

SPLforConstWidthBand7dB (scalar)

SPLforConstWidthBand8dB (scalar)

SPLforConstWidthBand9dB (scalar)

SPLforOctaveBandat125HzdB (scalar)

SPL for Octave Band at 125Hz (dB)

SPLforOctaveBandat16HzdB (scalar)

SPL for Octave Band at 16Hz (dB)

SPLforOctaveBandat16kHzdB (scalar)

SPL for Octave Band at 16kHz (dB)

SPLforOctaveBandat1HzdB (scalar)

SPL for Octave Band at 1Hz (dB)

SPLforOctaveBandat1kHzdB (scalar)

SPL for Octave Band at 1kHz (dB)

SPLforOctaveBandat250HzdB (scalar)

SPL for Octave Band at 250Hz (dB)

SPLforOctaveBandat2HzdB (scalar)

SPL for Octave Band at 2Hz (dB)

SPLforOctaveBandat2kHzdB (scalar)

SPL for Octave Band at 2kHz (dB)

SPLforOctaveBandat315HzdB (scalar)

SPL for Octave Band at .5Hz (dB)

SPLforOctaveBandat315kHzdB (scalar)

SPL for Octave Band at .5kHz (dB)

SPLforOctaveBandat4HzdB (scalar)

SPL for Octave Band at 4Hz (dB)

SPLforOctaveBandat4kHzdB (scalar)

SPL for Octave Band at 4kHz (dB)

SPLforOctaveBandat500HzdB (scalar)

SPL for Octave Band at 500Hz (dB)

SPLforOctaveBandat63HzdB (scalar)

SPL for Octave Band at 63Hz (dB)

SPLforOctaveBandat63kHzdB (scalar)

SPL for Octave Band at 63kHz (dB)

SPLforOctaveBandat8HzdB (scalar)

SPL for Octave Band at 8Hz (dB)

SPLforOctaveBandat8kHzdB (scalar)

SPL for Octave Band at 8kHz (dB)

SPLforOneThirdOctaveBandat125HzdB (scalar)

SPL for /-Octave Band at 125Hz

(dB)

SPLforOneThirdOctaveBandat125kHzdB (scalar)

(dB)

SPLforOneThirdOctaveBandat12p5HzdB (scalar)

(dB)

SPLforOneThirdOctaveBandat16HzdB (scalar)

SPL for /-Octave Band at 16Hz

(dB)

SPLforOneThirdOctaveBandat16kHzdB (scalar)

SPL for /-Octave Band at 16kHz

(dB)

SPLforOneThirdOctaveBandat25HzdB (scalar)

SPL for /-Octave Band at 25Hz

(dB)

SPLforOneThirdOctaveBandat25kHzdB (scalar)

SPL for /-Octave Band at 25kHz

(dB)

SPLforOneThirdOctaveBandat315HzdB (scalar)

SPL for /-Octave Band at 315Hz

(dB)

SPLforOneThirdOctaveBandat315kHzdB (scalar)

(dB)

SPLforOneThirdOctaveBandat31p5HzdB (scalar)

(dB)

SPLforOneThirdOctaveBandat63HzdB (scalar)

SPL for /-Octave Band at 63Hz

(dB)

SPLforOneThirdOctaveBandat63kHzdB (scalar)

SPL for /-Octave Band at 63kHz

(dB)

(dB)

(dB)

(dB)

SSTF1BlendingFunction (scalar)

SST F1 Blending Function

SSTF2BlendingFunction (scalar)

SST F2 Blending Function

SaturationPressure (scalar)

Saturation Pressure

SaturationRatio (scalar)

Saturation Ratio

SaturationTemperature (scalar)

Saturation Temperature

ScalarDissipation (scalar)

Scalar Dissipation

ScatteringCoefficient (scalar)

Scattering Coefficient

SchmidtNumber (scalar)

Schmidt Number

SecondaryMeanMixtureFraction (scalar)

Secondary Mean Mixture Fraction

SecondaryMixtureFractionVariance (scalar)

Secondary Mixture Fraction Variance

SensibleEnthalpy (scalar)

Sensible Enthalpy

SensitivityToViscosity (scalar)

Sensitivity To Viscosity

SensitivitytoBodyForceXComponent (scalar)

Sensitivity to Body Force

X-Component

SensitivitytoBodyForceXComponentCellValues

(scalar)

X-Component (Cell Values)

SensitivitytoBodyForceYComponent (scalar)

Y-Component

SensitivitytoBodyForceYComponentCellValues

(scalar)

Y-Component (Cell Values)

SensitivitytoBodyForceZComponent (scalar)

Z-Component

SensitivitytoBodyForceZComponentCellValues

(scalar)

Z-Component (Cell Values)

SensitivitytoBoundaryHeatFlux (scalar)

Sensitivity to Boundary Heat Flux

SensitivitytoBoundaryPressure (scalar)

Sensitivity to Boundary Pressure

SensitivitytoBoundaryTemperature (scalar)

Sensitivity to Boundary Temperature

SensitivitytoBoundaryVelocity (vector)

Sensitivity to Boundary %s-Velocity

SensitivitytoEnergySources (scalar)

Sensitivity to Energy Sources

SensitivitytoEnergySourcesCellValues (scalar)

Sensitivity to Energy Sources (Cell

Values)

SensitivitytoFlowBlockage (scalar)

Sensitivity to Flow Blockage

SensitivitytoMassSources (scalar)

Sensitivity to Mass Sources

SensitivitytoMassSourcesCellValues (scalar)

Sensitivity to Mass Sources (Cell

Values)

ShapeSensitivityComponent (vector)

Shape Sensitivity %s Component

ShapeSensitivityMagnitude (scalar)

Shape Sensitivity Magnitude

ShieldingFunctionforSBESorSDES (scalar)

Shielding Function for SBES or SDES

SkewSizeCavMarkType (scalar)

Skew/Size Cav. Mark Type

SkewSizeCavMarking (scalar)

Skew/Size Cav. Marking

SkewSizeCavSeeds (scalar)

Skew/Size Cav. Seeds

SkinFrictionCoefficient (scalar)

Skin Friction Coefficient

SmoothedCurvature (scalar)

Smoothed Curvature

SmoothedVOF (scalar)

Smoothed VOF

SmoothedVOFGradientMagnitude (scalar)

Smoothed VOF Gradient Magnitude

SmoothedVOFGradientd (vector)

Smoothed VOF Gradient-d%s

SolarBINID (scalar)

Solar BIN ID

SolarHeatFlux (scalar)

Solar Heat Flux

SolidusTemperature (scalar)

Solidus Temperature

SolvedTurbulentKineticEnergyk (scalar)

Solved Turbulent Kinetic Energy (k)

SoundPotential (scalar)

Sound Potential

SoundPressure (scalar)

Sound Pressure

SoundSpongeLayerMarker (scalar)

Sound Sponge Layer Marker

SoundWaveEqAp (scalar)

Sound WaveEq Ap

SoundWaveEqModelSource (scalar)

Sound WaveEq Model Source

SoundWaveEqModelSourceMask (scalar)

Sound WaveEq Model Source Mask

SoundWaveEqModelSourceSmoothed (scalar)

Smoothed

SoundWaveEqReconstructiondVard (vector)

Sound WaveEq Reconstruction

dVar/d%s

SoundWaveEqSource (scalar)

Sound WaveEq Source

SoundWaveEqdVard (vector)

Sound WaveEq dVar/d%s

Soundd2Pdt2 (scalar)

Sound d2P/dt2

SounddPdt (scalar)

Sound dP/dt

SourceTerm (scalar with species)

%s Source Term

SourcesofDQMOMm4 (scalar)

Sources of DQMOM-m4

SourcesofDQMOMvof (scalar)

Sources of DQMOM-vof

SparkDiffusionMultiplier (scalar)

Spark Diffusion Multiplier

SparkHeatSource (scalar)

Spark Heat Source

SpatialSpectralBandwidth (scalar)

Spatial Spectral Bandwidth

SpecDissAp (scalar)

Spec Diss Ap

SpecDissSource (scalar)

Spec Diss Source

SpeciesTurbulentTimeScale (scalar)

Turbulent Time Scale

SpecificDissipationRateOmega (scalar)

Specific Dissipation Rate (Omega)

SpecificEnthalpy (scalar)

Enthalpy

SpecificEntropy (scalar)

Entropy

SpecificHeatCapacity (scalar)

Specific Heat (Cp)

SpecificHeatRatiogamma (scalar)

Specific Heat Ratio (gamma)

SpecificHeatof (scalar with species)

Specific Heat of %s

SpecificInternalEnergy (scalar)

Internal Energy

SpecificTotalEnergy (scalar)

Total Energy

SpecificTotalEnthalpy (scalar)

Total Enthalpy

SpeedOfSound (scalar)

Sound Speed

SpinodalTemperature (scalar)

Spinodal Temperature

StaticPressure (scalar)

Static Pressure

StaticTemperature (scalar)

SteamDensityGasPhase (scalar)

Steam Density (Gas-Phase)

StoredElementPartition (scalar)

Stored Cell Partition

StrainRate (scalar)

Strain Rate

StretchFactor (scalar)

Stretch Factor

SubcooledVaporTemperature (scalar)

Subcooled Vapor Temperature

SubcriticalCondition (scalar)

Subcritical Condition

SubgridDissipationRate (scalar)

Subgrid Dissipation Rate

SubgridDynamicPrandtlNumber (scalar)

Subgrid Dynamic Prandtl Number

SubgridDynamicScof (scalar with species)

Subgrid Dynamic Sc of %s

SubgridDynamicScofFmean (scalar)

Subgrid Dynamic Sc of Fmean

SubgridDynamicScofProgressVariable (scalar)

Subgrid Dynamic Sc of Progress

Variable

SubgridDynamicViscosityConst (scalar)

Subgrid Dynamic Viscosity Const

SubgridEffectiveViscosity (scalar)

Subgrid Effective Viscosity

SubgridFilterLength (scalar)

Subgrid Filter Length

SubgridKineticEnergy (scalar)

Subgrid Kinetic Energy

SubgridTestFilterLength (scalar)

Subgrid Test-Filter Length

SubgridTurbulentViscosity (scalar)

Subgrid Turbulent Viscosity

SubgridTurbulentViscosityRatio (scalar)

Subgrid Turbulent Viscosity Ratio

SubtestKineticEnergy (scalar)

Subtest Kinetic Energy

SurfaceAcousticPower (scalar)

Surface Acoustic Power

SurfaceAcousticPowerLeveldB (scalar)

Surface Acoustic Power Level (dB)

SurfaceClusterID (scalar)

Surface Cluster ID

SurfaceHeatFlux (scalar)

Total Surface Heat Flux

SurfaceHeatTransferCoefficient (scalar)

Wall Func. Heat Tran. Coef.

SurfaceIncidentRadiation (scalar)

Surface Incident Radiation

SurfaceNusseltNumber (scalar)

Surface Nusselt Number

SurfaceStantonNumber (scalar)

Surface Stanton Number

SurfacedpdtRMS (scalar)

Surface dpdt RMS

TFMEfficiencyFactor (scalar)

TFM Efficiency Factor

TFMOmega (scalar)

TFM Omega

TFMThickeningFactor (scalar)

TFM Thickening Factor

TangentialVelocity (scalar)

Tangential Velocity

TemperatureAp (scalar)

Temperature Ap

TemperatureEMSurfaceSource (scalar)

Temperature EM Surface Source

TemperatureEMVolumeSource (scalar)

Temperature EM Volume Source

TemperatureSource (scalar)

Temperature Source

TemporalSpectralBandwidth (scalar)

Temporal Spectral Bandwidth

ThermalConductivity (scalar)

Thermal Conductivity

ThermalDiffCoefof (scalar with species)

Thermal Diff Coef of %s

ThinFilmHeatFlux (scalar)

Thin Film Heat Flux

TimeStep (scalar)

Time Step

TimeStepScale (scalar)

Time Step Scale

TotalEChemHeatSource (scalar)

Total EChem Heat Source

TotalEnthalpyDeviation (scalar)

Total Enthalpy Deviation

TotalFluctuationEnergy (scalar)

Total Fluctuation Energy

TotalPressure (scalar)

Total Pressure

TotalSurfaceCorrosionRate (scalar)

Total Surface Corrosion Rate

TotalTemperature (scalar)

Total Temperature

TransmittedIRSolarFlux (scalar)

Transmitted IR Solar Flux

TransmittedRadiationFlux (scalar)

Transmitted Radiation Flux

TransmittedVisibleSolarFlux (scalar)

Transmitted Visible Solar Flux

TurbDissAp (scalar)

Turb Diss Ap

TurbDissSource (scalar)

Turb Diss Source

TurbKinEnergyAp (scalar)

Turb Kin. Energy Ap

TurbKinEnergySource (scalar)

Turb Kin. Energy Source

TurbulenceDissipationRate (scalar)

Turbulent Dissipation Rate (Epsilon)

TurbulenceIntensity (scalar)

Turbulent Intensity

TurbulenceIntermittency (scalar)

Intermittency

TurbulenceViscosity (scalar)

Turbulent Viscosity

TurbulenceViscosityRatio (scalar)

Turbulent Viscosity Ratio

TurbulentFlameSpeed (scalar)

Turbulent Flame Speed

TurbulentFlameSpeedSource (scalar)

Turbulent Flame Speed Source

TurbulentKineticEnergyk (scalar)

Turbulent Kinetic Energy (k)

TurbulentLengthScale (scalar)

Turbulent Length Scale

TurbulentReynoldsNumberRe_t (scalar)

Turbulent Reynolds Number (Re_t)

TurbulentReynoldsNumberRe_y (scalar)

Turbulent Reynolds Number (Re_y)

TurbulentTimeScale (scalar)

TurbulentTimeStep (scalar)

Turbulent Time Step

TurbulentVelocityScale (scalar)

Turbulent Velocity Scale

TurbulentViscositylargescale (scalar)

Turbulent Viscosity (large-scale)

TurbulentViscositysmallscale (scalar)

Turbulent Viscosity (small-scale)

TwoLayerBlendingFunction (scalar)

Two Layer Blending Function

UCorrectionVelocity (scalar)

U Correction Velocity

UnNormalizedProgressVariable (scalar)

Un-Normalized Progress Variable

UnNormalizedProgressVariableVariance (scalar)

Variance

UnburntDensity (scalar)

Unburnt Density

UnburntFuelMassFraction (scalar)

Unburnt Fuel Mass Fraction

UnburntThermalDiffusivity (scalar)

Unburnt Thermal Diffusivity

UserEnergySource (scalar)

User Energy Source

UserMassSource (scalar)

User Mass Source

V2FTimeScale (scalar)

V2F Time Scale

VCorrectionVelocity (scalar)

V Correction Velocity

VOFAp (scalar)

VOF Ap

VOFGradientd (vector)

VOF Gradient-d%s

VOF Ap

VOFS (scalar)

VOF S

VaporPhaseHeatFlux (scalar)

Vapor Phase Heat Flux

VarianceofDistancefromFlame (scalar)

Variance of Distance from Flame

VelocityAngle (scalar)

Velocity Angle

VelocityDivergence (scalar)

Velocity Divergence

VelocityMagnitude (scalar)

Velocity Magnitude

VelocityVarianceScalev2 (scalar)

Velocity Variance Scale (v2)

ViscousConvectiveVariance (scalar)

Viscous-Convective Variance

ViscousDiffusiveVariance (scalar)

Viscous-Diffusive Variance

VolumeGlobFactor (scalar)

Volume Glob Factor

VolumeGlobSource (scalar)

Volume Glob Source

Volumefraction (scalar)

Volume fraction

VolumetricAbsorbedRadiation (scalar)

Volumetric Absorbed Radiation

VolumetricEmittedRadiation (scalar)

Volumetric Emitted Radiation

Vorticity (vector)

%s-Vorticity

VorticityMagnitude (scalar)

Vorticity Magnitude

WCorrectionVelocity (scalar)

W Correction Velocity

WallAdjacentHeatTransferCoef (scalar)

Wall Adjacent Heat Transfer Coef.

WallAdjacentTemperature (scalar)

Wall Adjacent Temperature

WallCoverage (scalar)

Wall Coverage

WallFilmFacePressGradient (vector)

Wall Film Face Press %s-Gradient

WallFilmFacePressure (scalar)

Wall Film Face Pressure

WallFilmHeatFlux (scalar)

Wall Film Heat Flux

WallFilmHeight (scalar)

Wall Film Height

WallFilmImpingementMassFlux (scalar)

Wall Film Impingement Mass Flux

WallFilmImpingementMomentum (vector)

Wall Film Impingement

%s-Momentum

WallFilmImpingementMomentumMag (scalar)

Wall Film Impingement Momentum

Mag

WallFilmMass (scalar)

Wall Film Mass

WallFilmMassM0 (scalar)

WallFilmTemperature (scalar)

Mag

Wall Film Temperature

WallFilmVelocity (vector)

Wall Film %s-Velocity

WallFilmVelocityMagnitude (scalar)

Wall Film Velocity Magnitude

WallIrradiationFluxNormalizedStdDeviation

(scalar)

Wall Irradiation Flux.Normalized Std

Deviation

WallTemperature (scalar)

Wall Temperature

WallTemperatureShellCellThin (scalar)

Wall Temperature (Shell Cell/Thin)

WallTemperatureThin (scalar)

Wall Temperature (Thin)

WallYplus (scalar)

Wall Yplus

WallYstar (scalar)

Wall Ystar

XFaceArea (scalar)

X Face Area

XVelocityMeshSmoothing (scalar)

X Velocity Mesh Smoothing

YFaceArea (scalar)

Y Face Area

YVelocityMeshSmoothing (scalar)

Y Velocity Mesh Smoothing

ZFaceArea (scalar)

Z Face Area

ZVelocityMeshSmoothing (scalar)

Z Velocity Mesh Smoothing

dHd (vector)

dH-d%s

dMassFractiondx (scalar with species)

dMass Fraction %s-dx

dMassFractiondy (scalar with species)

dMass Fraction %s-dy

dMassFractiondz (scalar with species)

dMass Fraction %s-dz

dSDRd (vector)

dSDR/d%s

dTEDd (vector)

dTED/d%s

dTKEd (vector)

dTKE/d%s

dTd (vector)

dT-d%s

dVelocitydz (vector)

d%s-Velocity/dz

ded (vector)

de-d%s

dkd (vector)

dk-d%s

dnutd (vector)

dnut-d%s

dpd (vector)

dp-d%s

dpdt (scalar)

dp-dt

drhod (vector)

drho-d%s

dvofd (vector)

dvof-d%s

log10ShapeSensitivityMagnitude (scalar)

log10(Shape Sensitivity Magnitude)

Chapter : Reading and Manipulating Meshes

ANSYS Fluent can import different types of meshes from various sources. You can modify the mesh by

translating or scaling node coordinates, partitioning the domain for parallel processing, and merging

or separating zones. You can convert all 3D meshes to polyhedral cells, except for pure hex meshes.

Hexahedral cells are preserved during conversion. You can also obtain diagnostic information on the

mesh, including memory usage and simplex, topological, and domain information. You can find out

the number of nodes, faces, and cells in the mesh, determine the minimum and maximum cell volumes

in the domain, and check for the proper numbers of nodes and faces per cell. These and other capabil-

ities are described in the following sections.

.. Mesh Topologies

.. Mesh Requirements and Considerations

.. Mesh Sources

.. Reference Frames

.. Non-Conformal Meshes

.. Overset Meshes

.. Reporting Mesh Statistics

.. Converting the Mesh to a Polyhedral Mesh

.. Modifying the Mesh

See Adapting the Mesh (p. ) for information about adapting the mesh based on solution data and

related functions, and Mesh Partitioning and Load Balancing (p. ) for details on partitioning the mesh

for parallel processing.

As an unstructured solver, ANSYS Fluent uses internal data structures to assign an order to the cells,

faces, and grid points in a mesh and to maintain contact between adjacent cells. Therefore, it does not

require i,j,k indexing to locate neighboring cells. This gives you the flexibility to use the best mesh to-

pology for your problem, as the solver does not force an overall structure or topology on the mesh.

For 2D meshes, quadrilateral and triangular cells are accepted, and for 3D meshes, hexahedral, tetrahedral,

pyramid, wedge, and polyhedral cells can be used. Figure . : Cell Types (p. ) depicts each of these

cell types. Both single-block and multi-block structured meshes, as well as hybrid meshes containing

quadrilateral and triangular cells or hexahedral, tetrahedral, pyramid, and wedge cells are acceptable.

ANSYS Fluent also accepts meshes with hanging nodes (that is, nodes on edges and faces that are not

vertices of all the cells sharing those edges or faces) and hanging edges (that is, edges on faces that

do not act as edges for both of the cells sharing those faces), although you may need to remove the

hanging nodes/edges from interior walls. See Hanging Node Adaption in the Theory Guide for information

about acceptable hanging nodes, and Removing Hanging Nodes/Edges (p. ) and Converting Cells

with Hanging Nodes / Edges to Polyhedra (p. ) for details on removing hanging nodes/edges. Meshes

with non-conformal boundaries (that is, meshes with multiple subdomains in which the mesh node

locations at the internal subdomain boundaries are not identical) are also acceptable. For details, see

Non-Conformal Meshes (p. ).

Figure . : Cell Types

Some examples of meshes that are valid for ANSYS Fluent are presented in Examples of Acceptable

Mesh Topologies (p. ). Different cell shapes and their face-node connectivity are explained in Face-

Node Connectivity in ANSYS Fluent (p. ). Choosing the Appropriate Mesh Type (p. ) explains how

to choose the mesh type that is best suited for your problem.

... Examples of Acceptable Mesh Topologies

ANSYS Fluent can solve problems on a wide variety of meshes.Figure . : Structured Quadrilateral

Mesh for an Airfoil (p. )-Figure . : Polyhedral Mesh (p. ) show examples of meshes that are

valid for ANSYS Fluent.

Reading and Manipulating Meshes

O-type meshes, meshes with zero-thickness walls, C-type meshes, conformal block-structured meshes,

multiblock structured meshes, non-conformal meshes, and unstructured triangular, tetrahedral, quad-

rilateral, hexahedral, and polyhedral meshes are all acceptable.

Note

Though ANSYS Fluent does not require a cyclic branch cut in an O-type mesh, it will accept

a mesh that contains one.

Figure . : Structured Quadrilateral Mesh for an Airfoil

Figure . : Unstructured Quadrilateral Mesh

Mesh Topologies

Figure . : Multiblock Structured Quadrilateral Mesh

Figure . : O-Type Structured Quadrilateral Mesh

Figure . : Parachute Modeled With Zero-Thickness Wall

Figure . : C-Type Structured Quadrilateral Mesh

Figure . : 3D Multiblock Structured Mesh

Figure . : Unstructured Triangular Mesh for an Airfoil

Figure . : Unstructured Tetrahedral Mesh

Figure . : Hybrid Triangular/Quadrilateral Mesh with Hanging Nodes

Figure . : Non-Conformal Hybrid Mesh for a Rotor-Stator Geometry

Figure . : Polyhedral Mesh

... Face-Node Connectivity in ANSYS Fluent

This section contains information about the connectivity of faces and their related nodes in terms of

node number and face number.

Face-node connectivity for the following cell shapes is explained here:

triangular (Figure . : Face and Node Numbering for Triangular Cells (p. ))

quadrilateral (Figure . : Face and Node Numbering for Quadrilateral Cells (p. ))

tetrahedral (Figure . : Face and Node Numbering for Tetrahedral Cells (p. ))

wedge (Figure . : Face and Node Numbering for Wedge Cells (p. ))

pyramidal (Figure . : Face and Node Numbering for Pyramidal Cells (p. ))

hex (Figure . : Face and Node Numbering for Hex Cells (p. ))

polyhedral (Figure . : An Example of a Polyhedral Cell (p. ))

This information is useful in interfacing with ANSYS Fluent.

.... Face-Node Connectivity for Triangular Cells

Figure . : Face and Node Numbering for Triangular Cells

Associated Nodes

Face

Face

Face

Face

.... Face-Node Connectivity for Quadrilateral Cells

Figure . : Face and Node Numbering for Quadrilateral Cells

Face

Face

Face

Face

Face

.... Face-Node Connectivity for Tetrahedral Cells

Figure . : Face and Node Numbering for Tetrahedral Cells

Face

--

Face

--

Face

--

Face

--

Face

.... Face-Node Connectivity for Wedge Cells

Figure . : Face and Node Numbering for Wedge Cells

Face

--

Face

---

Face

---

Face

---

Face

--

Face

.... Face-Node Connectivity for Pyramidal Cells

Figure . : Face and Node Numbering for Pyramidal Cells

Face

---

Face

--

Face

--

Face

--

Face

--

Face

.... Face-Node Connectivity for Hex Cells

Figure . : Face and Node Numbering for Hex Cells

Face

---

Face

---

--

Face

--

Face

--

Face

Face

---

Face

---

Face

---

Face

---

Face

---

Face

---

Face

.... Face-Node Connectivity for Polyhedral Cells

Figure . : An Example of a Polyhedral Cell

For polyhedral cells, there is no explicit face and node numbering as with the other cell types.

... Choosing the Appropriate Mesh Type

ANSYS Fluent can use meshes composed of triangular or quadrilateral cells (or a combination of the

two) in 2D, and tetrahedral, hexahedral, polyhedral, pyramid, or wedge cells (or a combination of these)

in 3D. The choice of which mesh type to use will depend on your application. When choosing mesh

type, consider the following issues:

setup time

computational expense

numerical diffusion

.... Setup Time

Many flow problems solved in engineering practice involve complex geometries. The creation of

structured or block-structured meshes (consisting of quadrilateral or hexahedral elements) for such

problems can be extremely time-consuming if not impossible. Therefore, setup time for complex

geometries is the major motivation for using unstructured meshes employing triangular or tetrahedral

cells. However, if your geometry is relatively simple, there may be no saving in setup time with either

approach.

Other risks of using structured or block-structured meshes with complicated geometries include the

oversimplification of the geometry, mesh quality issues, and a less efficient mesh distribution (for

example, fine resolution in areas of less importance) that results in a high cell count.

If you already have a mesh created for a structured code, it will save you time to use this mesh in

ANSYS Fluent rather than regenerate it. This can be a motivation for using quadrilateral or hexahedral

cells in your ANSYS Fluent simulation.

Note

ANSYS Fluent has a range of filters that allow you to import structured meshes from other

codes, including FLUENT . For details, see Mesh Sources (p. ).

.... Computational Expense

When geometries are complex or the range of length scales of the flow is large, a triangular/tetrahedral

mesh can be created with far fewer cells than the equivalent mesh consisting of quadrilateral/hexa-

hedral elements. This is because a triangular/tetrahedral mesh allows clustering of cells in selected

regions of the flow domain. Structured quadrilateral/hexahedral meshes will generally force cells to

be placed in regions where they are not needed. Unstructured quadrilateral/hexahedral meshes offer

many of the advantages of triangular/tetrahedral meshes for moderately-complex geometries.

A characteristic of quadrilateral/hexahedral elements that might make them more economical in some

situations is that they permit a much larger aspect ratio than triangular/tetrahedral cells. A large aspect

ratio in a triangular/tetrahedral cell will invariably affect the skewness of the cell, which is undesirable

as it may impede accuracy and convergence. Therefore, if you have a relatively simple geometry in

which the flow conforms well to the shape of the geometry, such as a long thin duct, use a mesh of

high-aspect-ratio quadrilateral/hexahedral cells. The mesh is likely to have far fewer cells than if you

use triangular/tetrahedral cells.

Converting the entire domain of your (tetrahedral) mesh to a polyhedral mesh will result in a lower

cell count than your original mesh. Although the result is a coarser mesh, convergence will generally

be faster, possibly saving you some computational expense.

In summary, the following practices are generally recommended:

For simple geometries, use quadrilateral/hexahedral meshes.

For moderately complex geometries, use unstructured quadrilateral/hexahedral meshes.

For relatively complex geometries, use triangular/tetrahedral meshes with wedge elements in the

boundary layers.

For extremely complex geometries, use pure triangular/tetrahedral meshes.

.... Numerical Diffusion

A dominant source of error in multidimensional situations is numerical diffusion (false diffusion). The

term false diffusion is used because the diffusion is not a real phenomenon, yet its effect on a flow

calculation is analogous to that of increasing the real diffusion coefficient.

The following comments can be made about numerical diffusion:

Numerical diffusion is most noticeable when the real diffusion is small, that is, when the situation is con-

vection-dominated.

All practical numerical schemes for solving fluid flow contain a finite amount of numerical diffusion.This

is because numerical diffusion arises from truncation errors that are a consequence of representing the

fluid flow equations in discrete form.

The second-order and the MUSCL discretization scheme used in ANSYS Fluent can help reduce the effects

of numerical diffusion on the solution.

The amount of numerical diffusion is inversely related to the resolution of the mesh.Therefore, one way

of dealing with numerical diffusion is to refine the mesh.

Numerical diffusion is minimized when the flow is aligned with the mesh.

This is the most relevant to the choice of the mesh. If you use a triangular/tetrahedral mesh, the

flow can never be aligned with the mesh. If you use a quadrilateral/hexahedral mesh, this situation

might occur, but not for complex flows. It is only in a simple flow, such as the flow through a long

duct, in which you can rely on a quadrilateral/hexahedral mesh to minimize numerical diffusion.

In such situations, it is advantageous to use a quadrilateral/hexahedral mesh, since you will be able

to get a better solution with fewer cells than if you were using a triangular/tetrahedral mesh.

If you would like higher resolution for a gradient that is perpendicular to a wall, you can create prism

layers with higher aspect ratios near the wall.

This section contains information about special geometry/mesh requirements and general comments

on mesh quality.

... Geometry/Mesh Requirements

... Mesh Quality

You should be aware of the following geometry setup and mesh construction requirements at the

beginning of your problem setup:

Axisymmetric geometries must be defined such that the axis of rotation is the  axis of the Cartesian co-

ordinates used to define the geometry (Figure . : Setup of Axisymmetric Geometries with the x Axis as

the Centerline (p. )).

Figure . : Setup of Axisymmetric Geometries with the x Axis as the Centerline

ANSYS Fluent allows you to set up periodic boundaries using either conformal or non-conformal periodic

zones. For conformal periodic boundaries, the periodic zones must have identical meshes.

The conformal periodic boundary zones can be created in the meshing mode of Fluent or GAMBIT

when you are generating the volume mesh. See the Fluent Meshing section of the User’s Guide or

the GAMBIT Modeling Guide for more information.

Although Fluent to create periodic boundaries that are conformal, as well as periodic interfaces that

are non-conformal; the latter is necessary if you created your mesh using a CAD package that is not

able to produce true periodic boundaries. For details on creating such interfaces, see Creating Peri-

odic Zones and Interfaces (p. ).

The quality of the mesh plays a significant role in the accuracy and stability of the numerical compu-

tation. Regardless of the type of mesh used in your domain, checking the quality of your mesh is es-

sential. One important indicator of mesh quality that ANSYS Fluent allows you to check is a quantity

referred to as the orthogonality. In order to determine the orthogonality of a given cell, the following

quantities are calculated for each face :

the normalized dot product of the area vector of a face (

) and a vector from the centroid of the cell to

the centroid of that face (

):

(.)

):

(.)

the centroid of the adjacent cell that shares that face ( ):

(.)

The minimum value that results from calculating Equation . (p. ) and Equation . (p. ) for all

of the faces is then defined as the orthogonality for the cell. Therefore, the worst cells will have an

Mesh Requirements and Considerations

orthogonality closer to  and the best cells will have an orthogonality closer to . Figure . : The

Vectors Used to Compute Orthogonality (p. ) illustrates the relevant vectors.

Figure . : The Vectors Used to Compute Orthogonality

Orthogonal Quality depends on cell type:

For tetrahedral, prism, and pyramid cells, the Orthogonal Quality is the minimum of the orthogonality and

(- cell skewness).

For hexahedral and polyhedral cells, the Orthogonal Quality is the same as the orthogonality.

Another important indicator of the mesh quality is the aspect ratio. The aspect ratio is a measure of

the stretching of a cell. It is computed as the ratio of the maximum value to the minimum value of

any of the following distances: the normal distances between the cell centroid and face centroids

(computed as a dot product of the distance vector and the face normal), and the distances between

the cell centroid and nodes. For a unit cube (see Figure . : Calculating the Aspect Ratio for a Unit

Cube (p. )), the maximum distance is ., and the minimum distance is ., so the aspect ratio is

.. This type of definition can be applied on any type of mesh, including polyhedral.

Figure . : Calculating the Aspect Ratio for a Unit Cube

To check the quality of your mesh, you can use the Report Quality button in the General task page:

Setup →

General → Report Quality

A message will be displayed in the console, such as the example that follows:

Orthogonal Quality ranges from  to , where values close to  correspond to low quality.

If you would like more information about the quality displayed in the console (including additional

quality metrics and the zones that have the cells with the lowest quality), set the mesh/check-

verbosity text command to  (valid values are , , ) prior to using the Report Quality button.

For information about how to improve poor quality cells, see Repairing Meshes (p. ).

When evaluating whether the quality of your mesh is sufficient for the problem you are modeling, it

is important to consider attributes such as mesh element distribution, cell shape, smoothness, and

flow-field dependency. These attributes are described in the sections that follow.

.... Mesh Element Distribution

Since you are discretely defining a continuous domain, the degree to which the salient features of

the flow (such as shear layers, separated regions, shock waves, boundary layers, and mixing zones)

are resolved depends on the density and distribution of mesh elements. In many cases, poor resolution

in critical regions can dramatically affect results. For example, the prediction of separation due to an

adverse pressure gradient depends heavily on the resolution of the boundary layer upstream of the

point of separation.

Resolution of the boundary layer (that is, mesh spacing near walls) also plays a significant role in the

accuracy of the computed wall shear stress and heat transfer coefficient. This is particularly true in

laminar flows where the mesh adjacent to the wall should obey

(.)

where

= distance to the wall from the adjacent cell centroid

= free-stream velocity

= kinematic viscosity of the fluid

= distance along the wall from the starting point of the boundary layer

Equation . (p. ) is based upon the Blasius solution for laminar flow over a flat plate at zero incid-

ence [] (p. ).

Proper resolution of the mesh for turbulent flows is also very important. Due to the strong interaction

of the mean flow and turbulence, the numerical results for turbulent flows tend to be more susceptible

to mesh element distribution than those for laminar flows. In the near-wall region, different mesh

resolutions are required depending on the near-wall model being used. See Model Hierarchy (p. )

for guidelines.

In general, no flow passage should be represented by fewer than  cells. Most cases will require many

more cells to adequately resolve the passage. In regions of large gradients, as in shear layers or mixing

zones, the mesh should be fine enough to minimize the change in the flow variables from cell to cell.

Unfortunately, it is very difficult to determine the locations of important flow features in advance.

Moreover, the mesh resolution in most complicated 3D flow fields will be constrained by CPU time

and computer resource limitations (that is, memory and disk space). Although accuracy increases with

larger meshes, the CPU and memory requirements to compute the solution and postprocess the

results also increase. Solution-adaptive mesh refinement can be used to increase and/or decrease

mesh density based on the evolving flow field, and therefore provides the potential for more econom-

ical use of grid points (and hence reduced time and resource requirements). See Adapting the

Mesh (p. ) for information on solution adaption.

.... Cell Quality

The quality of the cell (including its orthogonal quality, aspect ratio, and skewness) also has a signi-

ficant impact on the accuracy of the numerical solution.

Orthogonal quality is computed for cells using cell skewness and the vector from the cell centroid to each

of its faces, the corresponding face area vector, and the vector from the cell centroid to the centroids of

each of the adjacent cells (see Equation . (p. ), Equation . (p. ), and Figure . :The Vectors Used

to Compute Orthogonality (p. )).The worst cells will have an orthogonal quality closer to , with the

best cells closer to .The minimum orthogonal quality for all types of cells should be more than ., with

an average value that is significantly higher.

Aspect ratio is a measure of the stretching of the cell. As discussed in Computational Expense (p. ), for

highly anisotropic flows, extreme aspect ratios may yield accurate results with fewer cells. Generally, it is

best to avoid sudden and large changes in cell aspect ratios in areas where the flow field exhibit large

changes or strong gradients.

Skewness is defined as the difference between the shape of the cell and the shape of an equilateral cell

of equivalent volume. Highly skewed cells can decrease accuracy and destabilize the solution. For example,

optimal quadrilateral meshes will have vertex angles close to  degrees, while triangular meshes should

preferably have angles of close to  degrees and have all angles less than  degrees. A general rule is

that the maximum skewness for a triangular/tetrahedral mesh in most flows should be kept below .,

with an average value that is significantly lower. A maximum value above . may lead to convergence

difficulties and may require changing the solver controls, such as reducing under-relaxation factors and/or

switching to the pressure-based coupled solver.

Cell size change and face warp are additional quality measure that could affect stability and accuracy.

See the Fluent Meshing section of the User’s Guide for more details.

.... Smoothness

Truncation error is the difference between the partial derivatives in the governing equations and their

discrete approximations. Rapid changes in cell volume between adjacent cells translate into larger

truncation errors. ANSYS Fluent provides the capability to improve the smoothness by refining the

mesh based on the change in cell volume or the gradient of cell volume. For information on marking

cells by cell volume and then refining the mesh, see Volume (p. ) and Refining and Coarsen-

ing (p. ).

.... Flow-Field Dependency

The effect of resolution, smoothness, and cell shape on the accuracy and stability of the solution

ing (p. ).

process is dependent on the flow field being simulated. For example, very skewed cells can be tolerated

in benign flow regions, but can be very damaging in regions with strong flow gradients.

Since the locations of strong flow gradients generally cannot be determined a priori, you should strive

to achieve a high-quality mesh over the entire flow domain.

Since ANSYS Fluent can handle a number of different mesh topologies, there are many sources from

which you can obtain a mesh to be used in your simulation. You can generate a mesh using ANSYS

Meshing, the meshing mode of Fluent, Fluent Meshing, GAMBIT, GeoMesh, PreBFC, ICEM CFD, I-deas,

NASTRAN, PATRAN, ARIES, Mechanical APDL, CFX, or other preprocessors. You can also use the mesh

contained in a Fluent/UNS, RAMPANT, or FLUENT  case file. You can also prepare multiple mesh files

and combine them to create a single mesh.

... ANSYS Meshing Mesh Files

... Fluent Meshing Mode Mesh Files

... Fluent Meshing Mesh Files

... GAMBIT Mesh Files

... GeoMesh Mesh Files

... PreBFC Mesh Files

... ICEM CFD Mesh Files

... Using the fe2ram Filter to Convert Files

... Removing Hanging Nodes/Edges

... Fluent/UNS and RAMPANT Case Files

... FLUENT  Case Files

Mesh Sources

... Reading Multiple Mesh/Case/Data Files

... Reading Surface Mesh Files

You can use ANSYS Meshing to create your mesh. Follow the meshing procedure and export to the

ANSYS Fluent mesh format (see Fluent Mesh Export in the ANSYS Meshing User’s Guide for details).

To import the mesh into Fluent, use the File/Read/Mesh... ribbon tab item (as described in Reading

Mesh Files (p. )).

You can use the meshing mode of  Fluent (which was previously a stand-alone program named Fluent

Meshing) to create 3D unstructured triangular/tetrahedral meshes from boundary or surface meshes.

Switch to meshing mode and then follow the meshing procedure described in the Fluent Meshing

section of the User’s Guide. You can save your mesh using the File/Write/Mesh... menu item.

Then switch to the solution mode to set up the case file for the transferred mesh, or import the saved

mesh into a new Fluent session using the File/Read/Mesh... ribbon tab item (as described in Reading

For information about switching between meshing and solution modes, see Switching Between

Meshing and Solution Modes (p. ) in the Getting Started Guide.

Prior to version ., Fluent Meshing was a stand-alone product that was used to create 3D unstructured

triangular/tetrahedral meshes from boundary or surface meshes. Fluent Meshing has been integrated

as the Fluent meshing mode. To import meshes created by Fluent Meshing into Fluent, use the

File/Read/Mesh... ribbon tab item (as described in Reading Mesh Files (p. )).

You can use GAMBIT to create 2D and 3D structured/unstructured/hybrid meshes. To create any of

these meshes for ANSYS Fluent, follow the procedure described in the GAMBIT Modeling Guide, and

export your mesh in Fluent / format. All such meshes can be imported directly into ANSYS Fluent using

the File/Read/Mesh... ribbon tab item, as described in Reading Mesh Files (p. ).

You can use GeoMesh to create complete 2D quadrilateral or triangular meshes, 3D hexahedral meshes,

and triangular surface meshes for 3D tetrahedral meshes. To create any of these meshes for ANSYS

Fluent, follow the procedure described in the GeoMesh User's Guide.

To complete the generation of a 3D tetrahedral mesh, read the surface mesh into the meshing mode

of Fluent and generate the volume mesh there (see the Fluent Meshing section of the User’s Guide

for details). All other meshes can be read directly into the solution mode of Fluent. Use the

File/Read/Mesh... ribbon tab item to read the mesh files, as described in Reading Mesh Files (p. ).

You can use PreBFC to create two different types of meshes for ANSYS Fluent, structured quadrilater-

al/hexahedral and unstructured triangular/tetrahedral.

.... Structured Mesh Files

To generate a structured 2D or 3D mesh, follow the procedure described in the PreBFC User's

Guide (Chapters  and ). The resulting mesh will contain quadrilateral (2D) or hexahedral (3D) elements.

Do not specify more than  wall zones and  inlet zones.

To import the mesh, use the File/Import/PreBFC File... ribbon tab item, as described in PreBFC

To manually convert a file in PreBFC format to a mesh file suitable for ANSYS Fluent, enter the following

command:

utility fl42seg input_filename output_filename

The output file produced can be read into ANSYS Fluent using the File/Read/Mesh... ribbon tab item,

as described in Reading Mesh Files (p. ).

.... Unstructured Triangular and Tetrahedral Mesh Files

To generate an unstructured 2D mesh, follow the procedure described in the PreBFC User's Guide.

Save the mesh file in the RAMPANT format using the MESH-RAMPANT/TGRID command. The current

ANSYS Fluent format is the same as the RAMPANT format. The resulting mesh will contain triangular

elements. To import the mesh, use the File/Read/Mesh... ribbon tab item, as described in Reading

Mesh Files (p. ).

To generate a 3D unstructured tetrahedral mesh, follow the procedure described in Chapter  of the

PreBFC User's Guide for generating a surface mesh. Then read the surface mesh into the meshing

mode of Fluent, and complete the mesh generation there. See the Fluent Meshing section of the

User’s Guide for details.

You can use ICEM CFD to create structured meshes in FLUENT  format and unstructured meshes in

RAMPANT format.

To import a FLUENT  mesh, follow the instructions in FLUENT  Case Files (p. ).

To import a RAMPANT mesh, use the File/Read/Mesh... ribbon tab item, as described in Reading Mesh

The current ANSYS Fluent format is the same as the RAMPANT format,not the FLUENT  format. After

reading a triangular or tetrahedral ICEM CFD volume mesh, improve its quality through smoothing (as

described in Quality-Based Smoothing (p. )).

You can import an I-deas Universal file into ANSYS Fluent in three different ways.

Generate an I-deas surface or volume mesh containing triangular, quadrilateral, tetrahedral, wedge and/or

hexahedral elements. Import it into the meshing mode of Fluent using the commands described in the

Fluent Meshing section of the User’s Guide. Adhere to the restrictions described in Appendix B: Mesh File

Format (p. ) in the Fluent Meshing section of the User’s Guide. In meshing mode, complete the mesh

generation (if necessary); then you can switch to the solution mode of Fluent or read it into a new Fluent

session as described in Fluent Meshing Mode Mesh Files (p. ).

Generate an I-deas volume mesh with linear triangular, quadrilateral, tetrahedral, wedge, or hexahedral

elements. Import it directly using the File/Import/I-deas Universal... ribbon tab item, as described in I-

deas Universal Files (p. ).

elements. Use the fe2ram filter to convert the Universal file to the format used by ANSYS Fluent.To convert

an input file in I-deas Universal format to an output file in ANSYS Fluent format, follow the instructions

below in Using the fe2ram Filter to Convert Files (p. ). After the output file is written, read it into ANSYS

Fluent using the File/Read/Mesh... ribbon tab item, as described in Reading Mesh Files (p. ).

.... Recognized I-deas Datasets

The following Universal file datasets are recognized by the ANSYS Fluent mesh import utility:

Node Coordinates dataset number , ,

Elements dataset number , ,

Permanent Groups dataset number , , , , ,

For 2D volume meshes, the elements must exist in a constant  plane.

Note

The mesh area or mesh volume datasets are not recognized. This implies that writing

multiple mesh areas/volumes to a single Universal file may confuse ANSYS Fluent.

.... Grouping Nodes to Create Face Zones

Nodes are grouped in I-deas using the Group command to create boundary face zones. In ANSYS

Fluent, boundary conditions are applied to each zone. Faces that contain the nodes in a group are

gathered into a single zone. It is important not to group nodes of internal faces with nodes of

boundary faces.

curve or mesh area will be a different zone in ANSYS Fluent. You may also create the groups manually,

generating groups consisting of all nodes related to a given curve (2D) or mesh area (3D).

.... Grouping Elements to Create Cell Zones

Elements in I-deas are grouped using the Group command to create the multiple cell zones. All ele-

ments grouped together are placed in a single cell zone in ANSYS Fluent. If the elements are not

grouped, ANSYS Fluent will place all the cells into a single zone.

.... Deleting Duplicate Nodes

I-deas may generate duplicate or coincident nodes in the process of creating elements. These nodes

must be removed in I-deas before writing the universal file for import into ANSYS Fluent.

There are three different ways in which you can import a NASTRAN file into ANSYS Fluent:

You can generate a NASTRAN surface or volume mesh containing triangular, quadrilateral, tetrahedral,

wedge, and/or hexahedral elements, and import it into the meshing mode of Fluent using the commands

described in the Fluent Meshing section of the User’s Guide. Adhere to the restrictions described in Ap-

pendix B: Mesh File Format (p. ) in the Fluent Meshing section of the User’s Guide. In meshing mode,

complete the mesh generation (if necessary); then you can switch to the solution mode of Fluent or read

it into a new Fluent session as described in Fluent Meshing Mode Mesh Files (p. ).

You can generate a NASTRAN volume mesh with linear triangular, quadrilateral, tetrahedral, wedge, or

hexahedral elements, and import it directly using the File/Import/NASTRAN ribbon tab item, as described

in NASTRAN Files (p. ).

hexahedral elements.Then use the fe2ram filter to convert the NASTRAN file to the format used by ANSYS

Fluent.To convert an input file in NASTRAN format to an output file in ANSYS Fluent format, follow the in-

structions below in Using the fe2ram Filter to Convert Files (p. ). After the output file has been written,

you can read it into ANSYS Fluent using the File/Read/Mesh... ribbon tab item, as described in Reading

After reading a triangular or tetrahedral NASTRAN volume mesh using the latter methods, improve its

quality through smoothing (as described in Quality-Based Smoothing (p. )).

.... Recognized NASTRAN Bulk Data Entries

The following NASTRAN file datasets are recognized by the ANSYS Fluent mesh import utility:

GRID single-precision node coordinates

GRID* double-precision node coordinates

CBAR line elements

CTETRA, CTRIA3 tetrahedral and triangular elements

CHEXA, CQUAD4, CPENTA hexahedral, quadrilateral, and wedge elements

NASTRAN may generate duplicate or coincident nodes in the process of creating elements. These

nodes must be removed in NASTRAN before writing the file for import into ANSYS Fluent.

There are three different ways in which you can import a PATRAN Neutral file into ANSYS Fluent.

You can generate a PATRAN surface or volume mesh containing triangular, quadrilateral, tetrahedral,

You can generate a PATRAN volume mesh with linear triangular, quadrilateral, tetrahedral, wedge, or

hexahedral elements (grouping nodes with the same component-group name) and import it directly to

ANSYS Fluent by selecting the File/Import/PATRAN ribbon tab item, as described in PATRAN Neut-

ral Files (p. ).

hexahedral elements and then use the fe2ram filter to convert the Neutral file into the format used by

ANSYS Fluent.To convert an input file in PATRAN Neutral format to an output file in ANSYS Fluent format,

follow the instructions below in Using the fe2ram Filter to Convert Files (p. ). After the output file has

been written, you can read it into ANSYS Fluent using the File/Read/Mesh... ribbon tab item, as described

in Reading Mesh Files (p. ).

After reading a triangular or tetrahedral PATRAN volume mesh using the latter methods, improve its

Important

To retain a zone type during PATRAN Neutral file import, add the abbreviated form of the

“zone-type” before the “zone-name”, as shown below:

Zone Name for PATRAN export (zone-type) - (zone-name)

Zone Type in ANSYS Fluent

m-f-i-zone-name

p-o-zone-name

fan-zone-name

fan

v-i-zone-name

p-f-f-zone-name

solid-zone-name

solid

fluid-zone-name

fluid

.... Recognized PATRAN Datasets

The following PATRAN Neutral file packet types are recognized by the ANSYS Fluent mesh import

utility:

Node Data Packet Type

Element Data Packet Type

Distributed Load Data Packet Type

Node Temperature Data Packet Type

Name Components Packet Type

File Header Packet Type

Elements are grouped in PATRAN using the Named Component command to create the multiple

cell zones. All elements grouped together are placed in a single cell zone in ANSYS Fluent. If the

elements are not grouped, ANSYS Fluent will place all the cells into a single zone.

There are three different ways in which you can import a Mechanical APDL file into ANSYS Fluent.

You can generate a surface or volume mesh containing triangular, quadrilateral, tetrahedral, wedge, or

hexahedral elements using Mechanical APDL or ARIES, and import it into the meshing mode of Fluent using

the commands described in the Fluent Meshing section of the User’s Guide. Adhere to the restrictions de-

scribed in Appendix B: Mesh File Format (p. ) in the Fluent Meshing section of the User’s Guide. In

meshing mode, complete the mesh generation (if necessary); then you can switch to the solution mode

of Fluent or read it into a new Fluent session as described in Fluent Meshing Mode Mesh Files (p. ).

You can generate a Mechanical APDL volume mesh with linear triangular, quadrilateral, tetrahedral, wedge,

or hexahedral elements, as well as with higher order elements like  node hexahedron, SOLID92, and

SOLID187.Then import it directly to ANSYS Fluent using the File/Import/Mechanical APDL ribbon tab

item, as described in Mechanical APDL Files (p. ).

The higher order elements will be converted to their corresponding linear elements during the import in

or hexahedral elements, and then use the fe2ram filter to convert the Mechanical APDL file into the format

used by ANSYS Fluent.To convert an input file in ANSYS . or . format to an output file in ANSYS Flu-

ent format, follow the instructions in Using the fe2ram Filter to Convert Files (p. ). After the output file

has been written, you can read it into ANSYS Fluent using the File/Read/Mesh... ribbon tab item, as described

After reading a triangular or tetrahedral volume mesh using method  or  above, you should improve

its quality through smoothing (as described in Quality-Based Smoothing (p. )).

.... Recognized ANSYS . and . Datasets

ANSYS Fluent can import mesh files from ANSYS . and . (.cdb files), retaining original boundary

names. The following ANSYS file datasets are recognized by the ANSYS Fluent mesh import utility:

NBLOCK node block data

EBLOCK element block data

CMBLOCK element/node grouping

You can import the meshes from 3D CFX files, such as definition (.def) and result (.res) files into

ANSYS Fluent, using the File/Import/CFX ribbon tab item, as described in CFX Files (p. ). The fe2ram

utility is used as the import filter, which can be used as a stand-alone program to obtain an ANSYS

Fluent mesh file. See Using the fe2ram Filter to Convert Files (p. ) for information about fe2ram.

Important

Important

Note that you have the ability to import only the mesh from a CFX file, and not any results

or data.

When importing a mesh from a CFX  definition or results file, select whether you want the ANSYS

Fluent zones to be created from the physics data objects or the primitive mesh region objects. The

former option is the default and is called “Zoning by CCL” and the latter option is called “Zoning by

Group”. This will allow you to choose the type of mesh topology you would like to preserve when

importing the file:

If you want zones to be created from the physics data objects, enable Create Zones from CCL Physics

Data in the Select File dialog box.

If you want zones to be created from the primitive mesh region objects, disable Create Zones from CCL

Physics Data in the Select File dialog box.This will result in the group zoning.

Important

The primitive mesh topology may contain additional regions that do not appear in the

physics definition.

The default import method is the Create Zones from CCL Physics Data method. This method will

not import CFX subdomain regions, however, the zoning by group method can import subdomain

regions.

The 3D element set corresponding to zones/domains present in these files are imported as cell zones

in ANSYS Fluent. They may contain tetrahedral, pyramidal, wedge, and hexahedral elements. The

boundary zones in these files are a group of faces with a boundary condition name/type and are im-

ported as face zones with the boundary condition name/type retained in ANSYS Fluent. The following

boundary condition types are retained:

inlet

outlet

symmetry

interface

wall

inlet

outlet

symmetry

interface

wall

The boundaries of type Interface may be conformal or non-conformal. If they are non-conformal,

they are retained. However, conformal interfaces contain coincident nodes that are merged and changed

to type Interior. For some cases, for the merge to work correctly, the merge tolerance may need

to be adjusted. Alternatively, the Fuse Face Zones Dialog Box (p. ) in ANSYS Fluent can be used to

merge the conformal interfaces. For details, see Fusing Face Zones (p. ).

The fe2ram filter can be used to manually convert files of certain formats into ANSYS Fluent mesh

files, which can then be read into ANSYS Fluent. To use the fe2ram filter, enter the following at a

command prompt in a terminal or command window:

utility fe2ram [dimension] format [zoning] input_file output_file

Note

The items enclosed in square brackets are optional. Do not type the square brackets.

dimension indicates the dimension of the dataset. Replace dimension with -d2 to indicate that the mesh

is two dimensional. For a 3D mesh, do not enter any value for dimension, because 3D is the default.

format indicates the format of the file you want to convert. For example, replace format with -tANSYS for

a Mechanical APDL file, -tIDEAS for an I-deas file, -tNASTRAN for a NASTRAN file, and so on.To print a

list of the formats which fe2ram can convert, type

utility fe2ram -cl -help.

Note

fe2ram does not support VRML . or later.

zoning indicates how zones were identified in the original format. Replace zoning by -zID for a mesh that

was zoned by property IDs, or -zNONE to ignore all zone groupings. For a mesh zoned by group, do not

enter anything for zoning, because zoning by groups is the default.

input_file is the name of the original file. output_file is the name of the file to which you want to write the

converted mesh information.

For example, if you wanted to convert the 2D I-deas volume mesh file sample.unv to an output

file called sample.grd, you will enter the following command:

utility fe2ram -d2 -tIDEAS sample.unv sample.grd

As noted in Mesh Topologies (p. ), ANSYS Fluent can accept meshes that contain hanging nodes or

hanging edges. However, the creation of interior walls can yield an error if hanging nodes/edges are

located on the zone that is turned into an interior wall. This problem can occur in the following cases:

If you read a mesh file that has an interior (or two-sided) wall boundary condition setup, but the shadow

wall has not been created yet.

If you turn an interior surface into a wall.

If you slit an interior surface (for example, turn it into a non-conformal interface).

Such error-producing hanging nodes / edges may be present in hexcore or CutCell meshes, for example.

You can remove the hanging nodes/edges by converting the associated cells to polyhedra. Each cell

that is converted will retain the same overall dimensions, but the number of faces associated with the

cell will increase. You have the option of reading the mesh in the meshing mode of Fluent and then

writing it with the Write As Polyhedra option enabled; alternatively, you could read it in the solution

mode of Fluent and use the mesh/polyhedra/convert-hanging-nodes text command.

.... Limitations

Meshes with polyhedra have the following limitations:

The following mesh manipulation tools are not available on polyhedral meshes:

– extrude-face-zone under the modify-zone option

– skewness smoothing

– swapping (will not affect polyhedral cells)

The polyhedral cells that result from the conversion are not eligible for adaption with the default hanging

node method, though they can be refined with the polyhedral unstructured mesh adaption (PUMA)

method. For more information about adaption, see Adapting the Mesh (p. ).

The polyhedral cells that result from this conversion have the following limitations with regard to the

update methods available for dynamic mesh problems:

– When applying dynamic layering to a cell zone, you cannot have polyhedral cells adjacent to the moving

face zone.

– None of the remeshing methods except for CutCell zone remeshing will modify polyhedral cells.

Note that smoothing is allowed for polyhedral cells, and diffusion-based smoothing is recommended

over spring-based smoothing (see Diffusion-Based Smoothing (p. ) for details). The linearly

elastic solid smoothing method is not compatible with polyhedral cells.

If you have a Fluent/UNS  or  case file or a RAMPANT , , or  case file and you want to run an

ANSYS Fluent simulation using the same mesh, you can read it into ANSYS Fluent using the

File/Read/Case... ribbon tab item, as described in Reading Fluent/UNS and RAMPANT Case and Data

If you have a FLUENT  case file and you want to run an ANSYS Fluent simulation using the same mesh,

import it into ANSYS Fluent using the File/Import/FLUENT  Case File... ribbon tab item, as described

in Fluent  Case Files (p. ). ANSYS Fluent will read mesh information and zone types from the FLUENT

case file.

Important

FLUENT  may interpret some pressure boundaries differently from the current release of

ANSYS Fluent. Check the conversion information printed out by ANSYS Fluent to see if you

need to modify any boundary types.

To manually convert an input file in FLUENT  format to an output file in the current ANSYS Flu-

ent format, enter the following command:

After the output file has been written, you can read it into ANSYS Fluent using the File/Read/Case...

ribbon tab item, as described in Reading Mesh Files (p. ).

If you have an ANSYS FIDAP Neutral file and you want to run an ANSYS Fluent simulation using the

same mesh, import it using the ribbon item, as described in ANSYS FIDAP Neutral Files (p. ). ANSYS

Fluent will read mesh information and zone types from the ANSYS FIDAP file.

To manually convert an input file in ANSYS FIDAP format to an output file in ANSYS Fluent

utility fe2ram [ dimension ] -tFIDAP7 input_file output_file

The item in square brackets is optional. Do not type the square brackets. For a 2D file, replace dimension

with -d2. For a 3D file, do not enter anything for dimension, because 3D is the default.

After the output file has been written, read it into ANSYS Fluent using the File/Read/Case... ribbon

tab item, as described in Reading Mesh Files (p. ).

There may be some cases in which you will need to read multiple mesh files (subdomains) to form

your computational domain.

To solve on a multiblock mesh, generate each block of the mesh in the mesh generator and save it to a

separate mesh file.

For very complicated geometries, it may be more efficient to save the mesh for each part as a separate

mesh file.

The mesh node locations need not be identical at the boundaries where two separate meshes meet.

ANSYS Fluent can handle non-conformal mesh interfaces. See Non-Conformal Meshes (p. ) for details

about non-conformal mesh boundaries.

There are three ways of reading multiple mesh files in ANSYS Fluent:

Read multiple mesh files into the solution mode of Fluent.

Read multiple mesh files into the meshing mode of Fluent.

Use tmerge to manipulate the individual files and merge them into a single file that can then be read into

Fluent.

.... Reading Multiple Mesh Files via the Solution Mode of Fluent

The solution mode of Fluent allows you to handle more than one mesh at a time within the same

solver settings. This capability of handling multiple meshes saves time, since you can directly read in

the different mesh files and start setting up the solution, without having to switch over from meshing

mode or employ another tool such as tmerge.

The steps to take when reading more than one mesh file are:

. Read in your first mesh file.

In The Select File Dialog Box (p. ) (Figure . : The Select File Dialog Box (p. )), select the

mesh file and click OK.

. Read in your second mesh file and append it to the first mesh selected in the first step.

Domain → Zones → Append → Append Case File...

In The Select File Dialog Box (p. ), select the second mesh file and click OK.

. (optional). Display your meshes using the Mesh Display dialog box.

Setup →

General → Display...

You will find that the second mesh is appended to the first.

ANSYS Fluent also allows you to append the data on the mesh. To do that, follow the procedure

above. For the second step, use the following ribbon tab item:

Domain → Zones → Append → Append Case & Data Files...

Select the case file in The Select File Dialog Box (p. ) (Figure . : The Select File Dialog Box (p. )),

and click OK. Both the case and data files will be appended.

Important

Review your case setup after appending multiple mesh and/or data files before proceeding

with the calculation.

.... Reading Multiple Mesh Files via the Meshing Mode of Fluent

. Generate the mesh for the whole domain in the mesh generator, and save each cell zone (or block or

part) to a separate mesh file for Fluent.

Important

If one (or more) of the meshes you want to import is structured (for example, a FLUENT

mesh file), first convert it to ANSYS Fluent format using the fl42seg filter described

in FLUENT  Case Files (p. ).

. In the meshing mode of Fluent, combine the meshes into one mesh file.

a.

Read all of the mesh files. As the mesh files are read, they will be automatically merged into a single

mesh.

b. Save the merged mesh file.

a.

mesh.

See the Fluent Meshing section of the User’s Guide for information about reading and writing

files in meshing mode.

. Switch over to the solution mode of Fluent or read the combined mesh file into a new session using the

File/Read/Mesh... ribbon tab item.

For a conformal mesh, if you do not want a boundary between the adjacent cell zones, use the Fuse

Face Zones dialog box to fuse the overlapping boundaries. For details, see Fusing Face Zones (p. ).

The matching faces will be moved to a new zone with a boundary type of interior and the original

zone(s) will be discarded.

Important

If you are planning to use sliding meshes, or if you have non-conformal boundaries between

adjacent cell zones, do not combine the overlapping zones. Instead, change the type of

the two overlapping zones to interface (as described in Non-Conformal Meshes (p. )).

.... Reading Multiple Mesh Files via tmerge

part) to a separate mesh file for ANSYS Fluent.

Important

. Before launching Fluent, use the tmerge filter to combine the meshes into one mesh file.The tmerge

method allows you to rotate, scale, and/or translate the meshes before they are merged. Note that the

tmerge filter allows you to merge large meshes with very low memory requirement.

a.

a.

For 3D problems, type utility tmerge -3d. For 2D problems, type utility tmerge -2d.

b. When prompted, specify the names of the input files (the separate mesh files) and the name of the

output file in which to save the complete mesh. Be sure to include the .msh extension.

c.

For each input file, specify scaling factors, translation distances, and rotation information.

For information about the various options available when using tmerge, type utility tmerge

h.

. Read the combined mesh file into the solution mode of Fluent in the usual manner (using the

File/Read/Mesh... ribbon tab item).

Important

In this example, scaling, translation, or rotation is not requested. Hence you can simplify the inputs

to the following:

user@mymachine:> utility tmerge -2d

Starting /ansys_inc/v195/fluent/fluent19../utility/tmerge/lnamd64/tmerge_2d

Append 2D grid files.

tmerge2D ANSYS Inc, stream

Enter name of grid file (ENTER to continue) :  my1.msh

x,y scaling factor, eg. :

x,y translation, eg. :

rotation angle (deg), eg. :

Enter name of grid file (ENTER to continue) :  my2.msh

Enter name of grid file (ENTER to continue) :  {Enter}

Enter name of output file            : final.msh

Reading...

node zone: id , ib , ie , typ

.

.

.

done.

Writing...

nodes, id , ib , ie , type .

.

.

.

done.

Appending done.

Surface meshes are used as background meshes for geometry-based adaption. Perform the following

steps to read the surface mesh file into ANSYS Fluent:

. Open the Geometry Based Adaption dialog box.

Domain → Adapt → More → Geometry...

. Enable the Reconstruct Geometry option.

. Click the Surface Meshes... button to open the Surface Meshes dialog box (Figure . :The Surface

Meshes Dialog Box (p. )).

. In the Surface Meshes Dialog Box (p. ), click Read... and select the surface mesh file using The Select

File Dialog Box (p. ).

Specify the units the mesh was created in (default is meters).

Note that you can also display and delete the surfaces using Figure . : The Surface Meshes Dialog

Box (p. ).

Figure . : The Surface Meshes Dialog Box

You can create multiple local reference frames for use in setting up ANSYS Fluent cases.

The reference frames feature allows you to create local coordinate systems with a given position and

orientation, either with or without motion. Without local reference frames, you would have to specify

things such as surfaces based on the global reference frame/coordinate system.

... Creating and Using Reference Frames

To create a reference frame:

. Open the Reference Frame dialog box by right-clicking Reference Frames in the outline view and selecting

New....

Setup → Reference Frames

New...

Figure . : The Reference Frame Dialog Box

. Enter a Name for the reference frame.

. Specify how you want to define the reference frame.

User Defined allows you to completely specify the details of where the reference frame is located and

oriented and how it moves.

Track by Zone allows you to "attach" a reference frame to a cell zone.You can still specify where the

reference frame is located and how it is oriented, but you cannot specify any motion. If the zone it is

tracking moves, so does the reference frame.

. Specify either the Parent reference frame (when you select User Defined) or the Zone that the reference

frame will track (when you select Track by Zone.

. (Optional, User Defined only) enable Motion and specify the additional settings that appear in the Motion

tab.

Figure . : The Motion Tab of the Reference Frame Dialog Box

Linear Velocity is the linear velocity with respect to the parent reference frame orientation.

Rotational Velocity is the rotational velocity with respect to the parent reference frame orientation.

. Specify the Origin of your reference frame.

. Specify the orientation of the first axis of your reference frame in the Axis- Orientation group box. Select

which axis you are specifying using by selecting either the X, Y, or Z radio button. You can either specify

the orientation by providing a point or a direction.

. (Optional) Specify the orientation of the second axis of your reference frame. By default, Fluent automat-

ically provides an orientation for the second axis, but you can specify it manually by disabling Automatic

and providing your own inputs.

. Click OK to create the reference frame.

The Current State field shows you the current origin and axes directions of the reference frame with

respect to the global reference frame.

Using Reference Frames

You can use any local reference frame when defining point surfaces and profiles. Just select the desired

reference frame from the Reference Frame drop-down in the Point Surface or Profile dialog boxes.

Figure . : Point Surface Creation on Local Reference Frame

Figure . : Profile Definition on Local Reference Frame

In ANSYS Fluent it is possible to use a mesh that has non-conformal interfaces, that is, boundaries

between cell zones in which the mesh node locations are not identical. Such non-conformal interfaces

permit the cell zones to be easily connected to each other by passing fluxes from one mesh to another.

The principle requirement is that the boundary zones that make up the non-conformal interface must

overlap either partially or fully. (This requirement does not apply to non-conformal periodic boundaries.)

... Non-Conformal Mesh Calculations

... Non-Conformal Interface Algorithm

... Requirements and Limitations of Non-Conformal Meshes

... Using a Non-Conformal Mesh in ANSYS Fluent

Non-Conformal Meshes

To compute the flux across the non-conformal boundary, ANSYS Fluent must first compute the inter-

section between the interface zones that make up the boundary. In the case of a solid-to-solid zone

interface of the same material or a fluid-to-fluid zone interface, the resulting intersection produces an

interior zone where the two interface zones overlap (see Figure . : Completely Overlapping Mesh

Interface Intersection (p. )). In the case of a solid-to-solid zone interface of different materials or a

fluid-to-solid zone interface, the boundary is treated as a coupled wall (see The Coupled Wall Op-

tion (p. )).

Figure . : Completely Overlapping Mesh Interface Intersection

If one of the interface zones extends beyond the other (Figure . : Partially Overlapping Mesh Interface

Intersection (p. )), by default ANSYS Fluent will create additional wall zones for the portion(s) of the

boundary where the two interface zones do not overlap; these are referred to as "non-overlapping

zones", and can be changed to be other boundary conditions types at your discretion.

Figure . : Partially Overlapping Mesh Interface Intersection

Fluxes across the mesh interface are computed using the faces resulting from the intersection of the

two interface zones, not from the interface zone faces.

In the example shown in Figure . : Two-Dimensional Non-Conformal Mesh Interface (p. ), the in-

terface zones are composed of faces A-B and B-C, and faces D-E and E-F.

Figure . : Two-Dimensional Non-Conformal Mesh Interface

The intersection of these zones produces the faces a-d, d-b, b-e, and e-c. Faces produced in the region

where the two cell zones overlap (d-b, b-e, and e-c) are grouped to form an interior or coupled wall

zone (depending on the types of the adjacent cell zones), while the remaining face (a-d) forms a wall

zone.

To compute the flux across the interface into cell IV, face D-E is ignored and instead faces d-b and b-

e are used to bring information into cell IV from cells I and III.

While the previous discussion described the default treatment of a non-conformal interface, there are

several options you can enable at the interface in order to revise the treatment of the fluxes and/or

reduce the memory usage and processing time:

periodic boundary condition

periodic repeats

coupled wall

matching

mapped

static

These non-conformal interface options are described in the following sections.

....The Periodic Boundary Condition Option

....The Periodic Repeats Option

....The Coupled Wall Option

.... Matching Option

....The Mapped Option

....The Static Option

.... Interface Zones Automatic Naming Conventions

Non-conformal interfaces can be used to implement a periodic boundary condition like that described

for conformal periodic boundaries (see Periodic Boundary Conditions (p. )). The advantage of using

a mesh interface is that, unlike the standard periodic boundary condition, the nodes of the two zones

do not have to match one-for-one.

The interface zones that utilize the periodic boundary condition option (Figure . : Non-Conformal

Periodic Boundary Condition (Translational) (p. ) and Figure . : Non-Conformal Periodic Boundary

Condition (Rotational) (p. )) are coupled in the manner described in the previous section, except

that the zones do not overlap (that is, the zones are not spatially coincident at any point). In order

to generate the new faces that will be used to compute the fluxes across the interface, the nodes of

the first zone are either translated or rotated (about a given axis) onto the other zone. The dis-

tance/angle that the nodes are translated/rotated is called the “periodic offset”. The new faces will

be defined between all of the combined nodes, and then applied to each of the original zones.

Figure . : Non-Conformal Periodic Boundary Condition (Translational)

Figure . : Non-Conformal Periodic Boundary Condition (Rotational)

The periodic repeats option is appropriate when each of the interface zones is adjacent to a non-

conformal periodic interface or a pair of conformal periodic zones (see Figure . : Translational Non-

Conformal Interface with the Periodic Repeats Option (p. ) and Figure . : Rotational Non-Conformal

Interface with the Periodic Repeats Option (p. )). The periodic repeats option takes into account

the repeating nature of the flow solutions in the two cell zones in the following manner. Wherever

the interface zones overlap (that is, wherever interface zone  and  are spatially coincident), the

fluxes on either side of the interface are coupled in the usual way. The portion of interface zone

that does not overlap is coupled to the non-overlapping portion of interface zone , by translating

or rotating the fluxes by the periodic offset. This is similar to the treatment of non-conformal periodic

boundary conditions. The periodic repeats option is typically used in conjunction with the sliding

mesh model when simulating the interface between a rotor and stator.

Note

The periodic repeats option is not supported if the interface zone is adjacent to a solid

zone.

Figure . : Translational Non-Conformal Interface with the Periodic Repeats Option

Figure . : Rotational Non-Conformal Interface with the Periodic Repeats Option

As described previously, the typical function of non-conformal interfaces is to couple fluid zones, so

as to permit fluid flow to pass from one mesh interface to the other. Another available option is to

create a coupled wall boundary at the interface. In such a case, fluid flow would not pass across the

interface, as the interface is acting as a wall zone. Coupled wall heat transfer, on the other hand,

would be permitted. Such treatment is applied by default in the case of a solid-to-solid zone interface

of different materials or a fluid-to-solid zone interface. For fluid-to-fluid zone interfaces, you must

enable the Coupled Wall option to have such treatment; for example, you can model a thin wall or

baffle separating the two fluid zones. Figure . : Non-Conformal Coupled Wall Interfaces (p. ) illus-

trates coupled walls with both solid and fluid zones.

Note that coupled walls can also make use of the periodic repeats option. That is, both options can

be invoked simultaneously. For details see Using a Non-Conformal Mesh in ANSYS Fluent (p. ).

Figure . : Non-Conformal Coupled Wall Interfaces

When two interface zones do not match well (which could result from different mesh topologies,

geometric misalignment, or the existence of large gaps), wall zones will be created on the interface.

If, in such cases, you want to have only internal zones generated on the interface (that is, interior or

wall / shadow pairs), it is best to use a matching interface. If the interface zones are completely

overlapping (see Figure . : Completely Overlapping Mesh Interface Intersection (p. )) as opposed

to partially overlapping (see Figure . : Partially Overlapping Mesh Interface Intersection (p. )) and

so no wall zones are expected to be created on the mesh interface, it is recommended that you select

the Matching option.

Note

The Matching option is also compatible with the periodic boundary condition option.

Figure . : Matching Non-Conformal Wall Interfaces (p. ) below shows two interface zones that

do not match up well in the center -- the interface zone on the right has an inverted spike. Even with

such a large mismatch, the Matching option still enables you to create an interface with only the

interior zone.

Figure . : Matching Non-Conformal Wall Interfaces

When the Matching option is selected, ANSYS Fluent checks if one interface zone sits on top of the

other and displays messages if there is an overlap of cell zones that are connected through a mesh

interface (therefore making the interface invalid for use). Since the severity of zone overlap is different

for matching interfaces and non-matching interfaces, ANSYS Fluent displays different messages ac-

cordingly.

For example, for non-matching interfaces:

Info: Interface zones overlap for mesh interface (interface-name). This could adversely affect your solution.

Likewise, for matching interfaces:

Warning: Interface zone overlaps for mesh interface (interface-name).

This could generate left-handed faces on the interface and make it invalid for use.

The Mapped option is an alternative approach for modeling coupled walls between zones. This ap-

proach provides better handling for interface zones that penetrate each other or have gaps between

them. The Mapped option is useful in situations where using the standard non-conformal interface

formulations causes the simulation to fail (as may occur when there is interface penetration or gaps

between interfaces, causing the creation of left-handed faces at the interface).

Figure . : Non-Conformal Mapped Interface with a Gap and Penetration

Figure . : Non-Conformal Mapped Interface with a Gap and Penetration (p. ) shows significant

penetration between the two interface zones and large gap. The mapped option allows you to create

a coupled wall even with the large amount of penetration and gap shown in this image.

The Mapped option only works in conjunction with the Coupled Wall option. Enabling the Mapped

automatically enables Coupled Wall.

You can use the Interface Options Dialog Box (p. ) to modify the global settings for the mapped

interfaces, as well as to convert existing mesh interfaces (either all of them or just those that have

penetrating zones) to use the Mapped option.

You can confirm that you created good quality mapped interfaces by performing a mesh check. If

you have mapped interfaces that did not pass the quality check, Fluent will suggest that you use the

text command define/mesh-interface/improve-quality, which allows you to increase the

interface tolerance to improve the quality of the mapped interfaces.

In problems set up in version . or earlier, where you have a solid zone adjacent to a fluid zone

(conjugate heat transfer) with a mapped mesh interface between them, it is recommended you switch

from the explicit coupling method to the implicit method using the text command /define/mod-

els/cht/implicit-coupling?. The implicit method produces better convergence behavior

compared to the explicit method for these fluid-solid pairs. Note that the implicit method is the now

the default.

Note the following limitations when using the Mapped option:

The Mapped option can only be applied if at least one side of the interface consists of only solid zones.

The Mapped option is not compatible with shell conduction.

Thermal coupling calculations will not be performed at mapped interfaces for the Eulerian multiphase

model.

No other interface options besides Coupled Wall are allowed with the Mapped option.

For the S2S model, the Face to Face basis for the view factors is not compatible with mapped interfaces

for polyhedral meshes.

Mapped interfaces are not supported with the density-based solver.

Mapped interfaces are not supported with the Lagrangian discrete phase model.

Mapped interfaces are not supported with moving / deforming meshes.

For a default mesh interface or when the Coupled and/or Matching options are enabled, ANSYS

Fluent will automatically create zones that will be needed if the interface should change due to motion

(from moving reference frames or sliding meshes) or deformation. If you know in advance that the

interface zones will not be moving or deforming relative to each other at the interface, then (and

only then) it is recommended that you enable the Static option. The Static option prevents the creation

of such zones, and thus reduces the memory usage and processing time (for both the creation of the

interface and the running of the calculation). This reduction can be significant, especially when there

are many zones on both sides of the interface.

Warning

If the Static option is applied at an interface that does end up undergoing relative motion

or deformation, the results will be incorrect.

Note that the Static option is not limited to steady-state cases.

The following sub-sections describe the automatic naming conventions for each type of non-conformal

interface. Note that in these descriptions:

<mesh interface name> is user specified

<connection number side > is a value between  and m, where m is the number of zones in interface zone

side

<connection number side > is a value between  and n, where n is the number of zones in interface zone

side

<side number> is  or

..... Default (No Options Enabled)

..... Periodic Boundary Condition

..... Periodic Repeats

..... Coupled Wall

..... Matching

..... Mapped

..... Static

The automatic naming convention for the non-overlapping zones is as follows: <interface zone name>

non-overlapping.

The automatic naming convention for interface wall zone side  is as follows: <mesh interface name>

wall1 - <connection number side > - <connection number side >.

wall1 - <connection number side > - <connection number side > - shadow.

The automatic naming convention for interface interior zones is as follows: <mesh interface name>

interior - <connection number side > - <connection number side >.

periodic.

periodic.

periodic.

> define/mesh-interfaces/list

List of Mesh Interfaces

Interface Name:     cw:

Interface Options:  Coupled

Description                         Name                 ID           Area          Area Percentage

---------------------------  ----------------------------  --------  -----------------  -----------------

Interface-Zone-                            a2               .

Interface-Zone-                            a1               .

Interface-Zone-                            b1               .

Non-Overlapping-Zone-Side-            b1-non-overlapping              . .%

Interface-Wall-Zone-               cw:-wall1--               . .%

Interface-Wall-Zone-        cw:-wall1---shadow               . .%

The automatic naming convention for interface wall zones is as follows: <mesh interface name> -

wall <side number> - <connection number side > - <connection number side >.

Interface Name:     map:

Interface Options:  Mapped

Description                         Name                  ID            Area          Area Percentage

Interface-Wall-Zone-               map:-wall1-a2               . .%

Interface-Wall-Zone-               map:-wall1-a1               . .%

Interface-Wall-Zone-               map:-wall2-b1               . .%

The Static option does not affect the naming conventions of the zones; that is, the zone names will

be based entirely on the other settings in the Interface Options group box.

In the current version of ANSYS Fluent, non-conformal interface calculations are handled using one of

three approaches depending on the type of interface. Coupled Wall interfaces are handled using in-

terface boundary metrics and Mapped interfaces use a projection approach. The interface boundary

metrics and projection approach are both robust algorithms that avoid creating left-handed faces and

are particularly useful when you have complex geometries.

The remaining types of non-conformal interfaces are handled using a virtual polygon approach. The

virtual polygon approach stores the area vector and centroid of the polygon faces. This approach does

not involve node movement and cells are not necessarily water-tight cells. Hence gradients are corrected

to take into account the missing face area. Note that in transient cases, the stationary non-conformal

interfaces will be automatically preserved by ANSYS Fluent during mesh update.

Previous versions (. and earlier) of Fluent used the virtual polygon approach for all non-conformal

interfaces. The interface boundary metrics is a more robust approach for creating coupled wall interfaces

than the virtual polygon approach because it avoids creating left-handed faces. Older versions of Fluent

(. or earlier) used a triangular face approach, which triangulated the polygon intersection faces and

stored triangular faces. This approach involved node movement and water-tight cells, and was not as

stable as the virtual polygon approach. Note that case files created in releases prior to . can be

read and run normally in the current version of Fluent unless you recreate any of the interfaces. Recre-

ated coupled wall interfaces will use interface boundary metrics and all other recreated interfaces will

use the virtual polygon approach.

It is possible that distorted meshes may be produced during sliding mesh calculations, generating left-

handed faces. You cannot obtain a flow solution until all of the faces are “right handed”, and so ANSYS

Fluent corrects the left-handedness of these faces automatically. In extreme cases, the left-handed

faces cannot be fully corrected and are deleted automatically, so that the solution does not diverge.

Left-handed cells can also be created for the geometries that contain sharp edges and corners, which

may affect the final solution. For such geometries, you should first separate the zones and then create

the interfaces separately to get the better solution.

The additional input of the angle/translation vector at the angle/translation-vector prompt

in the console may be required to recreate face-periodic interfaces. Also, with the current mesh interface

algorithm in parallel, there is no need for encapsulation.

This section describes the requirements and limitations of non-conformal meshes:

The mesh interface can be of any shape (including a non-planar surface, in 3D), provided that the two in-

terface boundaries are based on the same geometry. If there are sharp features (for example, -degree

angles) or curvature in the mesh, it is especially important that both sides of the interface closely follow

that feature.

For example, consider the case of two concentric circles that define two fluid zones with a circular,

non-conformal interface between them, as shown in Figure . : A Circular Non-Conformal Inter-

face (p. ). Because the node spacing on the interface edge of the outer fluid zone is coarse com-

pared to the radius of curvature, the interface does not closely follow the feature (in this case, the

circular edge.)

Important

The maximum tolerance between two interfaces should not be larger than their adjacent

cell size at that location That is no cell should be completely enclosed between two inter-

faces.

Figure . : A Circular Non-Conformal Interface

If you create a single mesh with multiple cell zones separated by a non-conformal boundary, you must be

sure that each cell zone has a distinct face zone on the non-conformal boundary.

The face zones for two adjacent cell zones will have the same position and shape, but one will cor-

respond to one cell zone and one to the other. It is also possible to create a separate mesh file for

each of the cell zones, and then merge them as described in Reading Multiple Mesh/Case/Data

All periodic zones must be correctly oriented (either rotational or translational) before you create the non-

conformal interface.

In order for the periodic boundary condition option or periodic repeats option to be valid, the edges of

the second interface zone must be offset from the corresponding edges of the first interface zone by a

uniform amount (either a uniform translational displacement or a uniform rotation angle).This is not true

for non-conformal interfaces in general.

The periodic boundary condition option has the additional requirement that the angle associated

with a rotationally periodic must be able to divide  without remainder.

The periodic repeats option requires that some portion of the two interface zones must overlap (that is,

be spatially coincident).

The periodic repeats option requires that the non-overlapping portions of the interface zones must have

identical shape and dimensions. If the interface is part of a sliding mesh, you must define the mesh motion

such that this criterion is met at all times.

Note that for 3D cases, you cannot have more than one pair of conformal periodic zones adjacent to each

of the interface zones.

You must not have a single non-conformal interface where part of the interface is made up of a coupled

two-sided wall, while another part is not coupled (that is, the normal interface treatment). In such cases,

you must break the interface up into two interfaces: one that is a coupled interface, and the other that is

a standard fluid-fluid interface. See Using a Non-Conformal Mesh in ANSYS Fluent (p. ) for information

about creating coupled interfaces.

For simulations that involve the Fluent, Mechanical, and Meshing applications, meshing problems can arise

in instances where there are multiple regions and contacts between them. In Fluent, a zone can only exist

in a single contact region.The Mechanical and Meshing applications both use a different approach con-

cerning contact regions when compared to Fluent.

Fluid zones designated as 3D fan zones cannot have non-conformal interfaces.

If your multiple-zone mesh includes non-conformal boundaries, check if the mesh meets all the require-

ments (listed in Requirements and Limitations of Non-Conformal Meshes (p. )). This ensures that

ANSYS Fluent can obtain a solution on the mesh. Then do the following:

. Read the mesh into ANSYS Fluent. If you have multiple mesh files that have not yet been merged, first

follow the instructions in Reading Multiple Mesh/Case/Data Files (p. ) to merge them into a single mesh.

. For all of the zones that make up the non-conformal boundaries, change the type to interface (as described

in Changing Cell and Boundary Zone Types (p. )).

Setup →

Boundary Conditions

. Open the Mesh Interfaces Dialog Box (p. ) (Figure . :The Mesh Interfaces Dialog Box (p. )).

Setup → Mesh Interfaces

New...

Figure . : The Mesh Interfaces Dialog Box

. Create all of the mesh interfaces that use the periodic or periodic repeat option.This must be done using

the manual method, by clicking the Manual Create... button and using the Create/Edit Mesh Interfaces

Dialog Box (p. ). For details, see Manually Creating Mesh Interfaces (p. ).

. Create all of the mesh interfaces that do not use the periodic or periodic repeat option, using the automatic

method. As part of this method, Fluent will automatically determine which of the selected interface

boundary zones can be grouped together to form the two sides of one or more mesh interfaces.

To use the automatic method, perform the following steps in the Mesh Interfaces dialog box:

a.

a.

Select all of the zones in the selection list in the Unassigned Interface Zones group box.This list

contains only those zones that are not already part of an existing mesh interface. Note that you may

want to select only some of the zones when you want the resulting mesh interfaces to have different

name prefixes or different settings in the Auto Create Options dialog box (as described in the steps

that follow); for example, you could select only the interface zones from the front half of a model, and

then have all of the resulting mesh interfaces named with the prefix "front".

b. Enter the Interface Name Prefix you want applied to all of the resulting interfaces.

c.

(optional) Click the Options… button in the Unassigned Interface Zones group box to open the

Auto Create Options Dialog Box (p. ), and enable the settings that you want applied to all of the

resulting interfaces.

Figure . : The Auto Create Options Dialog Box

You can specify that all of the resulting interfaces are created using One to One Pairing, so that a

single zone is assigned to each side of all of the mesh interfaces. Using this option may decrease

your computational expense and help with troubleshooting later on, though it may produce a larger

number of mesh interfaces for you to manage.

Note that you can specify the proximity tolerance that ANSYS Fluent uses to determine which

zones should be grouped together as one-to-one interfaces. The proximity tolerance is defined

relative to the edge lengths in the interface zones, and can range from  to  (representing

the minimum and maximum edge lengths, respectively). Examples of when you may need

to adjust this setting from the default value of . include: when you have multiple mesh

interfaces that are close to each other (in which case you may need a smaller tolerance so

that the zones are not grouped erroneously); and when you have very small edges on an

interface zone (in which case you may need a larger tolerance so that the mesh interface is

identified). To revise the proximity tolerance, use the following text command:

define → mesh-interfaces → auto-options → proximity-tolerance

You can specify that the mapped option is applied to all of the resulting interfaces for which at least

one side of the interface consists of only solid zones, by enabling the Mapped option. Note that

the mapped option will be applied regardless of the mesh quality, and the tolerance used for

mapping will be that specified in the Interface Options Dialog Box (p. ). For more information

about the mapped option, see The Mapped Option (p. ).

You can specify that all of the resulting interfaces use the Static option, if and only if you know that

the interface zones will not be moving or deforming relative to each other at the interface.While

you will have the ability to enable the static option after the interfaces are created, doing so prior

to creation avoids the creation of unnecessary zones (and thus saves memory usage and processing

time, which can be significant when you have selected many Unassigned Interface Zones).

d. Click the Auto Create button in the Mesh Interfaces dialog box to create the interfaces.The resulting

interfaces will be added to the Mesh Interfaces list. Note that when all of the unassigned zones get

assigned, the Unassigned Interface Zones group box will become hidden, in order to simplify the

. If you need to revise any of the existing mesh interfaces (for example, if you want to enable the Coupled

Wall option), make a selection from the Mesh Interfaces list, click Edit..., and then complete the setup

in the Edit Mesh Interfaces Dialog Box (p. ) that opens.

Figure . : The Edit Mesh Interfaces Dialog Box

In the Edit Mesh Interfaces dialog box, select the Mesh Interfaces you want to change, revise

the settings, and click Apply. You can edit the Interface Name and/or the Interface Zones that

make up the interface (provided that the zones you select are unassigned and located appropriately),

though such changes are only allowed if you select a single interface. You can select one or more

interfaces and enable the following Interface Options; note that you can click the

button to

group the interfaces in the list by their currently enabled interface option(s), which allows you to

select / deselect all those of a particular type by simply clicking the top-level branch.

Enable Coupled Wall if you would like to model a thermally coupled wall between two fluid zones that

share a non-conformal interface.

Important

In the case of a solid-to-solid zone interface of different materials or a fluid-to-solid

zone interface, by default it is treated as a coupled wall. Therefore, no action is required

Important

in the Edit Mesh Interfaces dialog box to set up such an interface.

Enable the Matching option if only internal zones should be created (that is, interior or wall / shadow

pairs), since the interface zones on both sides are aligned.With the Matching option, even interface

zones that are not perfectly aligned are treated as if they are; however, if the discrepancy between the

interface zones on both sides exceeds default thresholds, then warning messages will be displayed.

See Matching Option (p. ) for more information about the recommended uses of this option.

Enable the Mapped option when there is penetration or large gaps between interface zones. Note that

at least one side of the interface must consist of only solid zones. For additional information, see The

Mapped Option (p. ).

Enable Enable Local Tolerance in the Mapped group box for the selected interface, if you want

to override the global tolerance defined for Mapped Tolerance in the Interface Options Dialog

Box (p. ).

Enable Static if and only if you know that the interface zones will not be moving or deforming relative

to each other at the interface.This option will reduce memory usage and processing time during the

running of the calculation, especially when there are many zones on both sides of the interface.The

only options it is compatible with are the Coupled Wall and/or Matching options. See The Static Op-

tion (p. ) for details.

The Periodic Boundary Condition and Periodic Repeats options are not available in the Edit Mesh

Interfaces dialog box, and so cannot be changed from enabled to disabled (or vice-versa) for an existing

interface; to change them, you must delete the interface and create it again with those options revised.

For interfaces that have the Periodic Boundary Condition option enabled, you can edit the Type and

Offset from the Edit Mesh Interfaces dialog box. Note that the Auto Compute Offset option must

be disabled to edit the Offset.

When all your changes are applied, close the Edit Mesh Interfaces dialog box.

. The buttons at the bottom of the Mesh Interfaces group box allow you to take further actions, such as

deleting or drawing a selected interface. Note the following:

The Delete button in the Mesh Interfaces dialog box can only be used on one mesh interface at a

time. If you would instead like to delete multiple interfaces in a single action, you can select them in

the tree and use the right-click menu command.

The Options... button opens the Interface Options Dialog Box (p. ), which allows you to update

which mesh interfaces use the mapped option and the related settings.

. Additional wall and interior zones will be created (and deleted) along with the mesh interfaces.

These zones will be named as described in Interface Zones Automatic Naming Conventions (p. ),

and are visible in the tree (for further details, see Interface Zones Automatic Naming Conven-

tions (p. )). There are times when you may need to take action on these additional zones, including

If the two interface zones did not overlap entirely, check the boundary zones created for the

non-overlapping portions to ensure that they are the proper boundary type and/or defined ap-

propriately. The non-overlapping zones are listed in the tree (as children of the associated interface

boundary zones), as well as in the relevant Interface dialog boxes. If the zone type is not correct,

you can use the Boundary Conditions Task Page (p. ) to change it; if the zone is not defined

appropriately, double-click it in the tree or click the Edit... button in the Interface dialog box,

and make the necessary changes in the dialog box that opens.

If you have any Coupled Wall type interfaces, define boundary conditions (if relevant) by updating the

interface wall zones using the Boundary Conditions task page.

Setup →

. It is always a good practice to initialize the solution and review your interfaces:

You can visualize the mesh interface(s) you have created by displaying contours of Mesh and Interface

Overlap Fraction in the Contours Dialog Box (p. ). See Figure . : Contours of Interface Overlap

Fraction (p. ) for an example.

Figure . : Contours of Interface Overlap Fraction

You can print information in the console about the areas of the zones associated with interfaces either

by using the List button in the Mesh Interfaces dialog box or by entering the text command

define/mesh-interface/list, as shown in the following example:

>define/mesh-interfaces/list

Interface Name:     int:

Description                       Name                 ID           Area         Area Percentage

---------------------------  ---------------------------  -------  ----------------  -----------------

Interface-Zone-                          f-             .

Interface-Zone-                          s-              .

Non-Overlapping-Zone-Side-          f--non-overlapping             . .%

Non-Overlapping-Zone-Side-          s--non-overlapping             . .%

Interface-Wall-Zone-             int:-wall1--             . .%

Interface-Wall-Zone-      int:-wall1---shadow             . .%

The Area Percentage for int:-side1-wall-f- is calculated as the area of int:-side1-wall-f-

divided by the area of f-. The Area Percentage for int:-wall1---shadow is calculated as

the area of int:-wall1---shadow divided by the area of s-. The remaining area percentages

are calculated in a similar manner.

. For dynamic meshes, by default any motion is automatically transferred across a mesh interface

when only one side is moving as a result of user-defined or system coupling motion, to ensure

that the coupling is maintained on both sides. To change the method by which the displacement

of the passive nodes is calculated or to disable this transfer altogether, use the define/mesh-

interfaces/transfer-motion-across-interfaces? text command.

With regard to the method by which the motion is transferred, you have two options: transfer-

displacements (the default) interpolates nodal displacement from the active side of the interface

to the passive side, and is recommended when there are gaps and/or penetrations in the mesh

interface that must be maintained; project-nodes projects the passive nodes onto the faces

of active side, and is recommended when the active side undergoes significant tangential motion

(as only the normal displacement is effectively transferred to the passive side in this method). For

further details, see Transferring Motion Across a Mesh Interface (p. ).

Note

For case files in which the interface was created in ANSYS Fluent version . or earlier, you

may reduce quality issues (such as left-handed faces) and/or convergence problems if you

recreate the interface in version . or later by entering the following Scheme command

in the console: (recreate-sliding-interfaces).

.... Manually Creating Mesh Interfaces

While it is possible to create every type of mesh interface using the manual method, it is only necessary

when you want your interface to use the periodic or periodic repeats option. For all other types it is

more convenient to use the automatic method (as described in the preceding section), especially

when you have many interface zones and/or are unfamiliar with their names / locations.

To manually create a mesh interface, you will use the Create/Edit Mesh Interfaces Dialog Box (p. ),

which is opened by clicking the Manual Create... button in the Mesh Interfaces Dialog Box (p. ).

Figure . : The Create/Edit Mesh Interfaces Dialog Box

. Enter a name for the interface in the Mesh Interface text-entry box.

. Specify the interface zones that make up the mesh interface by selecting one or more zones in the Inter-

face Zones Side  list and one or more zones in the Interface Zones Side  list. Note that you must select

only one zone per side if you plan to use the periodic or periodic repeats option.

Important

If one of your interface zones is much smaller than the other, you should specify the

smaller zone as Interface Zones Side  to improve the accuracy of the intersection

calculation.

. Enable the desired Interface Options:

Enable Periodic Boundary Condition to create a non-conformal periodic boundary condition interface.

– Select either Translational or Rotational as the periodic boundary condition Type to define the

type of periodicity.

– Retain the enabled default setting of Auto Compute Offset if you want ANSYS Fluent to automat-

ically compute the offset. After creating the interface, the offsets will be displayed in these fields.

The fields will be uneditable when the Auto Compute Offset is enabled.

– Disable Auto Compute Offset if you decide that you do not want ANSYS Fluent to find the offset.

In this case, you will have to provide the offset coordinates or angle in the required fields, depending

on whether Translational or Rotational periodicity is selected.

Important

→ Auto computation means that the rotational angle or the translational offset will be

automatically calculated and used while creating a non-conformal periodic boundary

condition interface. However, it still relies on the Rotational Axis Origin and the Ro-

tational Axis Direction that was entered for the cell zone in the cell zone condition

dialog box (for example, the Fluid dialog box).Therefore, before proceeding with the

creation of the non-conformal periodic boundary condition interface, you have to

correctly enter the rotational axis for the corresponding cell zone.

Note that auto computation of the non-conformal periodic boundary condition

offset does not mean that the Rotational Axis Origin and Rotational Axis

Direction are also detected automatically and updated. It is still your responsib-

ility to set up these values correctly.

→ For 3D cases, the Auto Compute Offset option requires that the periodic inter-

faces are connected by at least two face zones that meet at an edge that points

from one periodic zone to the other; this edge is used to calculate the offset. If

necessary, you can split a connecting zone into multiple zones in order to create

such an edge prior to creating the mesh interface.

Enable Periodic Repeats when each of the two cell zones has a single pair of conformal or non-con-

formal periodics adjacent to the interface (see Figure . :Translational Non-Conformal Interface with

the Periodic Repeats Option (p. )).This option is typically used in conjunction with the sliding mesh

model, when simulating the interface between a rotor and stator.

Other options are available, as described in the preceding section. Note that only Matching is compat-

ible with Periodic Boundary Condition, and only Coupled Wall is compatible with Periodic Repeats.

. Click Create/Edit... to create a new mesh interface. ANSYS Fluent will automatically create addi-

tional wall and/or interior zones for the interface, which will appear under Non-Overlapping

Zones Side , Non-Overlapping Zones Side , Interface Wall Zones Side , Interface Wall

Zones Side , and Interface Interior Zones.

. The buttons at the bottom of the dialog box allow you to take further actions, such as the following:

If you create an incorrect mesh interface, you can select it in the selection list and click the Delete

button to delete it. Any additional wall and/or interior zones that were created when the interface

was created will also be deleted.

To edit an interface, select it in the selection list and click Create/Edit..., and then revise the settings

using the Edit Mesh Interfaces Dialog Box (p. ) that opens.

You can click the Draw button to display interface zones or mesh interfaces in the graphics window.

Note that you can only select and display interface zones from Interface Zones Side  or Interface

Zones Side  if no interfaces are selected in the selection list and if the zone in question is not yet

assigned to an interface. After an interface is defined, you can select the appropriate mesh interface

and click the Draw button to display the zones under Interface Zones Side  and Interface Zones

Side  together. Drawing is particularly useful if you want to check the location of the interface zones

prior to setting up a mesh interface.

....Transferring Motion Across a Mesh Interface

ANSYS Fluent allows motion to be specified on either side of a mesh interface, and in some instances,

can transfer the motion from one side of a mesh interface to the other. When motion is specified on

one side of the interface (but not on the other) using either User-Defined Motion (p. ) or System

Coupling Motion (p. ), by default ANSYS Fluent will automatically interpolate and transfer this

motion so that the coupling is maintained on both sides. To disable this transfer or change the

method by which the displacement of the nodes on the passive side is calculated, use the following

text command:

define → mesh-interfaces → transfer-motion-across-interfaces?

When such transfer is disabled, the sides of the mesh interface may separate and/or penetrate over

the course of the simulation, which may lead to convergence difficulties and/or an invalid mesh.

When it is enabled, you have the following options:

the transfer-displacements approach (default)

This approach interpolates nodal displacement from the active side of the interface to the passive

side; it uses an inverse-distance weighted interpolation, so that the closer active nodes have more

influence. This may be beneficial in situations where gaps and/or penetrations are present at the

interface, and they need to be maintained as the simulation progresses. Note that any motion

specified tangential to the interface will also be interpolated to the passive side, which can lead

to unintended mesh dragging.

Figure . : Transferring Displacements

the project-nodes approach

This approach projects the nodes of the passive side of the interface onto the faces of the active

side, in order to maintain conformity. It is beneficial in situations that involve significant tangential

motions on the active side of the interface, as only the normal displacement is effectively transferred

to the passive side. Note that for mesh interfaces that involve significant gaps or penetration, the

project-nodes approach may cause the mesh to become invalid.

Figure . : Projecting Nodes

Note

If you expect the motion to produce large displacements, you should consider applying a

mesh update method on the cell zone of the passive side (such as smoothing or remeshing,

as described in Dynamic Mesh Update Methods (p. )).

Fluent allows you to build up the computational domain from overlapping meshes—also known as

Chimera or overset methodology. This gives you another way to build the complete mesh, in addition

to using conformally connected cell zones and non-conformal interfaces.

... Introduction

... Overset Topologies

... Overset Domain Connectivity

... Diagnosing Overset Interface Issues

... Overset Meshing Best Practices

... Overset Meshing Limitations and Compatibilities

... Setting up an Overset Interface

... Postprocessing Overset Meshes

...Writing and Reading Overset Files

Whereas non-conformal interfaces connect cell zones along matching face zones, overset interfaces

connect cell zones by interpolating cell data in the overlapping regions. For overset meshing to be

successful, the cell zones must overlap sufficiently. An advantage of overset meshing is that the indi-

vidual parts of an overset mesh can be generated independently and with fewer constraints than if

the parts had to fit together conformally or along non-conformal interfaces. This can make it easier to

replace parts of a mesh without having to remesh large parts or even the complete mesh.

Figure . : Overset Component and Background Mesh

Figure . : Overset Component and Background Mesh (p. ) shows a simplified mesh for a simulation

of flow over a cylinder in a duct. The mesh consists of two parts—a background mesh representing

the duct and a separate component mesh around the cylinder. The case is set up in Fluent as an

overset case by specifying the outer boundary of the cylinder mesh as overset (boundary type), and

by creating an overset interface containing the two cell zones. With these two steps complete, Fluent

automatically establishes the necessary connectivity between the meshes when the flow is initialized.

In this process, cells that fall outside the computational domain are classified as dead cells. The cells

where the flow equations are solved are referred to as solve cells. Receptor cells receive data interpolated

from another mesh. The donor cells—the cells where the receptors get their data—are a subset of the

solve cells. For the above case, Figure . : Solve Cells After Initialization (p. ) shows the solve cells

of the mesh after the flow is initialized. Note that in parallel, you can print partition statistics to get

information about some of the cell classifications, as described in Interpreting Partition Statistics (p. ).

Figure . : Solve Cells After Initialization

There is no limit on the number of cell zones that can be paired in an overset interface. Fluent classifies

the cell zones in an overset interface as either background or component:

Background zones are the cell zones that make up the background mesh of the computational domain.

They must be conformally connected and cannot have overset boundaries.

Component zones overlay background zones and have overset boundaries near where they connect to

the background and other component zones. Component zones can be conformally connected. If multiple

Overset Meshes

component zones are conformally connected, at least one of these zones needs to have an overset

boundary.

All cell types generally supported in Fluent are supported with overset meshing, including polyhedral

cells in 3D. The different zones paired in an overset interface can have different element types or can

have mixed element types.

Overset meshing in Fluent is compatible with mesh adaption. The mesh zones of an overset interface

can be locally adapted using all available adaption tools.

Overset meshing can be used for steady-state or transient solutions. Note that for steady-state cases

in parallel that use the default Metis partitioning, ANSYS Fluent will automatically repartition overset

meshes when the solution is initialized or data is read; a model-weighted partitioning that is designed

for optimal performance is used.

There are a multitude of configurations that can be constructed by superposing background and

component meshes in an overset interface. Fluent analyzes the topology of an interface with minimal

user input, which requires that the superposed meshes adhere to some topological constraints.

A case can have multiple overset interfaces, but a cell zone can only belong to a single interface. That

is, interfaces cannot share component or background meshes. It is always possible to have a single

overset interface for an entire model. However, it is more efficient to declare multiple interfaces if the

zonal topology allows it. Only including cell zones that are absolutely required in an interface also in-

creases efficiency.

In general, most overset interfaces will have at least one background and one component mesh.

However, ANSYS Fluent also allows you to set up overset interfaces that have no background mesh

and consist only of two or more component meshes.

An overset interface can contain multiple component and background meshes, provided that the

background meshes do not intersect each other.

Currently, non-conformal interfaces are not fully compatible with overset meshing. Component meshes

cannot be connected to a non-conformal interface and background meshes cannot have non-conformal

interfaces between them if they are part of the same overset interface.

The component meshes of an overset interface are allowed to overlap arbitrarily and multiple component

meshes can be combined to create an object of interest. However, an important topological constraint

is that physical boundary zones (wall, inlet, outlet, symmetry, and so on) are not allowed to intersect

each other. That is, a wall boundary cannot cross another wall boundary. For example, in the model

shown in Figure . : Overset Component and Background Mesh (p. ), the component mesh cannot

be placed such that its wall boundary zone intersects with the wall of the background mesh.

Overset boundaries can intersect with other overset boundaries and with physical boundaries. In Fig-

ure . : Overset Component and Background Mesh (p. ) the overset boundary of the component

mesh extends outside of the intended computational domain, crossing the wall boundary of the

background mesh—this is allowed. Figure . : Valid Overset Meshes with Components in Close

Proximity (p. ) shows a valid configuration of three cylinders in proximity (none of the physical

boundaries intersect with other physical boundaries).

Figure . : Valid Overset Meshes with Components in Close Proximity

Physical boundary zones are allowed to overlap, that is, a wall boundary (or parts of a wall boundary)

can be coincident with another wall boundary, as long as they do not cross. This powerful functionality

lets you build a body from overlapping parts or modify a body by adding parts. Figure . : Second

Component Modifying Existing Body (p. ) shows an overset configuration where a second component

mesh is added to an existing body to modify its shape. Fluent analyzes and automatically detects the

overlapping boundaries (walls in this case) of the different meshes in an overset interface, when deciding

which cells are solve cells and which cells are dead cells.

Figure . : Second Component Modifying Existing Body

Note that part of the wall boundary of mesh A lays on top of part of the wall boundary of mesh B, overlap-

ping it, but the walls do not cross or intersect.

Figure . : Existing Body Modification After Initialization (p. ) shows the solve cells of the mesh

after the flow field is initialized.

Figure . : Existing Body Modification After Initialization

The previous example shows a case where physical boundaries overlap between two component

meshes. Overlapping boundaries can also exist between component and background meshes.

If a body can only be built from components that have intersecting boundaries, then you must use a

collar mesh to properly connect them. A collar mesh is an additional component mesh that bridges

the intersecting physical boundaries, essentially transforming the intersection problem (not allowed)

into a problem of overlapping boundaries (allowed). Figure . : Multiple Components Bridged by

Collars Meshes (p. ) shows an overset interface consisting of two component meshes that have in-

tersecting wall boundaries. Two collar meshes (labeled C and D) are manually created to correctly

define the connectivity where the wall boundaries of the original component meshes (labeled A and

B) intersect. The wall boundaries of meshes C and D overlap with the wall boundaries of meshes A

and B.

Figure . : Multiple Components Bridged by Collars Meshes

Figure . : Multiple Components with Collar Meshes Initialized (p. ) shows the resulting solve cells

after the flow is initialized. The collar meshes act as fillet meshes that place the actual boundary inter-

sections into the interior of the body and outside of the fluid domain.

Figure . : Multiple Components with Collar Meshes Initialized

Special considerations are required when you intend to add a fluid region that expands the bounds

of an existing region, as shown in Figure . : Adding Fluid to a Region Using Cut Control (p. ). In

this example, a duct (A) is modified by adding a cavity (B). The boundaries of the two meshes intersect,

and by default the lower boundary of the duct would cut off the added cavity. In order to avoid this,

you need to use cut control to specify that the duct wall is not cutting the cavity cell zone, and, similarly,

that the cavity boundary is not cutting into the duct cell zone. See Hole Cutting Control (p. ) for

details on the available cut controls. The resulting mesh for the duct / cavity example after initialization

is shown in Figure . : Cut Controlled Region After Initialization (p. ).

Figure . : Adding Fluid to a Region Using Cut Control

Figure . : Cut Controlled Region After Initialization

Baffles (coupled walls) are permissible in overset meshing—both in background and component

meshes.

When an overset interface is initialized, there are three main steps that Fluent completes to establish

connectivity between the participating zones:

.... Hole Cutting

.... Overlap Minimization

.... Donor Search

Hole cutting is the process by which cells lying outside of the flow region (that is, inside bodies and

outside of the computational domain) are marked as dead cells. This is achieved by marking all the

cells that are cut by physical boundary zones (wall, inlet, outlet, symmetry, and so on), and marking

seed cells determined to lie outside the flow region for subsequent flood filling of dead cells. The

result of this flood filling is a valid overset mesh with maximum mesh overlap.

Figure . : Overset Component and Background Meshes Before Hole Cutting (p. ) and Fig-

ure . : Overset Component and Background Meshes After Hole Cutting (p. ) show an overset

mesh before and after hole cutting. All of the background cells that are bounded or cut by the cylinder

wall are classified as dead during hole cutting. The maximum overlap mesh shown in Figure . : Over-

set Component and Background Meshes After Hole Cutting (p. ) is a valid overset mesh, however,

it may not be ideal. An overly large overlap between component and background meshes is compu-

tationally inefficient (the equations are solved in more cells than are necessary). Additionally, the cell

sizes of the overlapping meshes may vary greatly—this affects the data interpolation and is detrimental

to solution quality. Ideally meshes should transition in regions of similar resolution.

Figure . : Overset Component and Background Meshes Before Hole Cutting

Figure . : Overset Component and Background Meshes After Hole Cutting

..... Hole Cutting Control

By default all boundary zones (other than overset boundaries) cut all other cell zones and mark dead

cells. If this is not the desired behavior (see Overset Topologies (p. )), you can manually specify

that a boundary zone does not cut certain cell zones. This optional cut control is available using the

following text command:

define → overset-interfaces → cut-control → add

A component mesh with only overset boundaries (for example, a refinement mesh zone overlaying

other zones) will cut into other mesh zones at its center and mark a single dead cell (cut seed) in

the overlaying mesh zones. This acts as a pilot hole that is then enlarged during the overlap minim-

ization. In cases where all cut boundaries of a component mesh are overlapping with other bound-

aries, you can force cut seeds in all component zones using the following text command:

define → overset-interfaces → cut-control → cut-seeds → cut-seeds-for-all-

component-zones?

Cut seeds are automatically enabled for all component zones when a cut control is added.

Overlap minimization is used to minimize mesh overlap among different component and background

meshes by converting additional solve cells into receptor cells and turning unnecessary receptors

into dead cells. During this process, a solve cell is turned into a receptor cell if the cell can find a

suitable donor cell with higher donor priority. By default, smaller cells have a higher donor priority.

Thus, in mesh overlap areas, without additional user input the solver attempts to obtain the solution

on the finest local mesh. The resulting mesh interface moves to an area where the meshes are more

comparable in cell size, leading to better solution quality. Figure . : Overset Component and Back-

ground Meshes After Overlap Minimization (p. ) shows the cylinder case from the previous figure

after the overlap minimization step.

Figure . : Overset Component and Background Meshes After Overlap Minimization

Note that overlap minimization is not literally minimizing the mesh overlap. The overlap minimization

is based on a flood filling of receptor cells, wherever suitable solve cells with higher donor priority

can be found. The resulting actual mesh overlap depends on the local donor priority distribution.

Also note that with overlap minimization, data interpolation between cell zones does not necessarily

occur at the overset boundaries. The purpose of specifying an overset boundary is primarily to specify

that overset mesh coupling should happen, and not where it should occur.

You have the option to specify different donor priority methods in order to control the location of

the overset interface. The text user interface command define/overset-interfaces/op-

tions/donor-priority-method allows you to specify that the donor priority is based either

on the cell size (proportional to the inverse of the cell volume) or the boundary distance (proportional

to the inverse of the distance to the closest boundary). Overlap minimization with donor priority

based on cell size (default) works best if the component mesh resolution is fine near walls and increases

away from walls, to spacings similar to—or larger than—the background mesh (see Figure . : Overset

Component and Background Meshes Before Hole Cutting (p. ) for an example of this type of mesh).

If the overlapping meshes have uniform and nearly identical resolutions, then overlap minimization

based on cell size will not reduce the overlap and a donor priority based on the boundary distance

should be used instead. The following two figures illustrate an overset mesh before and after initial-

ization where a donor priority based on boundary distance is used. Note that for the evaluation of

donor priorities based on boundary distance, all boundaries (including inlets, outlets, and so on) are

used for the distance evaluation.

Figure . : Overset Mesh Before Hole Cutting

Figure . : Overset Mesh After Minimization Based on Boundary Distance

You have the option for additional control over the overlap minimization process by assigning grid

priorities to component and background meshes, using the text user interface command

define/overset-interfaces/grid-priorities. Meshes (that is, cell zones) with higher

grid priorities are favored during the minimization process, irrespective of the local cell donor priority.

If two cell zones have the same grid priority, then the cell donor priorities are used for the overlap

minimization. For example, by assigning a higher grid priority to a coarser mesh, you can force Fluent

to minimize the finer mesh and obtain the solution on the coarser mesh, even if the donor priority

is based on cell size. Using grid priorities, similar to using donor priority based on boundary distance,

is helpful if local mesh distributions are irregular, and produce overlap regions that are irregular as

well. Note that the grid priorities take precedence over the donor priorities.

You have the option of disabling overlap minimization by using the text command define/overset-

interfaces/options/minimize-overlap?. This command is only available globally and applies

to all overset interfaces in the domain.

The donor search is the final step in establishing the domain connectivity. Fluent searches other

meshes for valid solve cells for each receptor. The solve cell containing the cell centroid of the receptor

cell, along with its connected solve cells, are used as donor candidates for a given receptor. Each re-

ceptor must have at least one valid donor cell.

There must be four or more cells in the overlap of both meshes to ensure a successful donor search.

The receptor cells, which form the fringe layer of a mesh zone, must overlap sufficiently with the

opposite mesh, such that they find valid solve cells as donors. For an example of valid mesh overlap,

see Figure . : Valid Overlap (p. ).

Figure . : Valid Overlap

Topology detection of overset interfaces in Fluent is automatic and does not require user input.

However, for it to work well, it requires that the provided meshes are of sufficient quality, particularly

when dealing with meshes that have overlapping boundaries.

Overset meshes are built from parts that can be meshed independently, which can lead people to

think of this as a much simpler process for mesh generation. This is not always the case, as considerable

thought is often required to generate good meshes for the individual components to avoid problems

during overset interface initialization.

If you are faced with issues during the initialization of an overset interface, there is most often no re-

covery without making changes to the mesh. You must analyze the cause of the issue, using the

available postprocessing and diagnostic tools, and improve the mesh before the simulation can con-

tinue.

When diagnosing overset interface failures, it can be convenient to use the text commands

define/overset-interfaces/intersect and define/overset-interfaces/clear

(available after enabling the expert tools available under define/overset-interfaces/op-

tions/expert) to execute and clear the hole cutting without having to initialize the solution.

The issues most often encountered are:

.... Flood Filling Fails During Hole Cutting

.... Donor Search Fails Due to Orphan Cells

These are the issues that can cause problems with flood filling:

..... Incorrect Seed Cells

..... Leakage Between Overlapping Boundaries

Flood filling of dead cells will fail if Fluent inadvertently identifies seed cells inside of the fluid zone

instead of outside. This can occur as a result of complexities in the topology or geometry of the

boundary zones, or because of mesh resolution issues. It manifests itself as an entire fluid region, or

a complete cell zone, being marked as dead.

This issue can be diagnosed by using the list command with the overset verbosity set to  (see

Overset Interface listing (p. )).

You can use the TUI command define/overset-interfaces/debug-hole-cut (available

after enabling the expert tools available under define/overset-interfaces/options/ex-

pert) to identify the problematic seed cells. This command allows you to execute the hole cutting

process on a specific overset interface and mark dead and seed cells.

When the flood fill option of the debug command is disabled, it will create two registers with dead

cells and seed cells which you can then display using the define/overset-interface/dis-

play-cells text command. The dead marks show the cells cut by the physical boundary zones.

The seed cells (mark0 register) show the cell candidates that will be used for flood filling.

If the flood fill option of the debug command is enabled, Fluent will then also create a register of

the seed cells from where flood filling actually started (mark1 register). If flood filling fails, displaying

these mark1 cells is the most efficient way to detect the problematic locations in the model.

It is critical that all the seed cells are located inside bodies or outside of the computational domain.

If there is a seed cell in the fluid region, it will cause a flood fill failure. It is not possible to recover

from flood filling failure without making changes to the model.

If no bad seed cells are found, as described in Incorrect Seed Cells (p. ), and there are overlapping

boundaries, it is likely that the overlapping boundaries do not match sufficiently and the flood filling

of dead cells leaks from the inside of the body to the outside. As a result, a complete cell zone can

disappear, due to having only dead cells. The permissible tolerance between overlapping boundary

zones is at most one cell-size in the wall normal direction. This can be restrictive when dealing with

prismatic boundary layer meshes with high cell aspect ratios at the wall. If your model suffers from

this leakage, you must improve the quality of the mesh, by making the overlapping boundary zones

match better.

If a receptor cell cannot find a valid donor cell, then it becomes an orphan cell. The presence of orphan

cells generally indicates that there is insufficient overlap between meshes or that the mesh resolutions

do not match well. As a result, the receptors are either finding no candidate donor cells, or invalid

candidates (dead or receptor cells).

Orphan cells can be an issue when walls of different meshes are in proximity. You must have at least

four cells in a gap, such as the ones between the walls in Figure . : Valid Overset Meshes with

Components in Close Proximity (p. ), in order to have a good connection between the

meshes—otherwise orphan cells are created. When a receptor overlays another receptor, it becomes

an orphan.

See Figure . : Invalid Overlap Creating Orphans (p. ) for an example of insufficient overlap causing

the creation of orphan cells. For information on visualizing orphan cells, see Postprocessing Overset

Meshes (p. ). Figure . : Valid Overlap (p. ) shows meshes overlapping sufficiently to avoid the

creation of orphan cells.

Figure . : Invalid Overlap Creating Orphans

You can mark the orphan cells, as described in Overset Cell Marks (p. ), which will likely indicate

where the mesh overlap must be increased. Sometimes, increasing the mesh resolution can lead to

a sufficient increase in mesh overlap. If mesh resolution is the issue, you can also use local mesh ad-

aption, along with mesh modification, to refine the mesh. Most often the mesh requiring adaption

is the mesh where the orphan should find its donors, and not the mesh zone containing the orphan.

If the presence of orphan cells in the simulation is unavoidable and you proceed with a calculation,

by default the solver applies a numerical treatment that attempts to assign reasonable values to the

orphan cells. This treatment has been found to prevent divergence in some instances, allowing the

solution to proceed; however, the orphan cell treatment does not guarantee the solution quality and

robustness a priori. The success of this treatment is case dependent, and difficult to predict based

on orphan cell counts. It is therefore highly recommended that you make every effort to eliminate

orphan cells by modifying the mesh, as described previously.

Receptor and donor cell sizes should be comparable to ensure that interpolation errors are minimized.

You can manually adapt the mesh to reduce the mismatch between donors and receptors.

You must have a minimum of four cells in a gap to create a valid overset interface, but a higher

number is recommended to ensure robust coupling between meshes and to prevent the creation of

orphan cells (see Figure . : Invalid Overlap Creating Orphans (p. ) and Figure . : Valid Over-

lap (p. )).

It is recommended that you start transient simulations from a converged steady-state solution.

lap (p. )).

If you are experiencing startup issues with a steady-state case, it is recommended that you ramp-up

to the final boundary conditions. For example, you can begin with a lower inlet velocity and a higher

viscosity to establish flow, before increasing to the target velocity and the desired final material

properties.

When using automatic timestep calculation for the pseudo-transient method, it is recommended that

you use the user-defined length scale option.

If you replace a zone that is part of an overset interface, you should either reinitialize the solution or

patch the solution on the replaced zone(s) before continuing with the calculation.

It is recommended that you use the double-precision solver for overset mesh simulations.

Closed domain cases are defined as setups that do not have a flow inlet or outlet boundary; this type

of setup is not supported with overset meshing if the working fluid is incompressible. If such a setup

is unavoidable, creating a small pressure-outlet boundary far away from the region of interest is recom-

mended before attempting to run the case using overset meshes.

For dynamic and sliding mesh cases, note the following:

The ideal time step size should be chosen such that the relative mesh motion does not exceed the

length of the smallest cell at the overset interface for a given time step.The mesh length used for

calculating the time step should be restricted to cells in the overset overlap region.This ensures a

more gradual evolution of the overset interface with the motion and is recommended for better ac-

curacy and stability.

In general, the motion of the overset interface may change the status for individual cells from dead

to receptor or solve, and vice versa.The exact instances depend on the relative mesh sizes of the

moving cell zones participating in the overset interface, the magnitude of the relative mesh velocity,

and the time step size.There is currently no mechanism to eliminate this type of cell status change

for general cases.

While the solver is capable of handling the cell status change, it is recommended that you actively

monitor these instances by setting the overset mesh verbosity to  using the define/overset-

interface/options/verbosity text command.With such a verbosity, the solver reports the

instances of dead to solve cells in the console. Keeping these to a minimum is highly recommended

for better accuracy and stability.

Do not have large variations in mesh resolution in the motion path that could trigger large changes

in the overset interface as the motion proceeds.The use of grid priorities can minimize large variations

in the overset interface.

You can specify that the overset interfaces use either the least squares interpolation method (the default)

or the inverse distance interpolation method by using the following text command.

solve → set → overset → interpolation-method

Overset meshing has the following limitations and compatibilities:

Overset meshing currently has the following limitations:

Overset interfaces cannot contain solid cell zones.

Component meshes cannot be connected to a non-conformal interface.

Background meshes cannot have non-conformal interfaces between them if they are part of the same

overset interface.

Component zones cannot have periodic boundary conditions.

Background zones cannot have overset boundaries.

Component mesh boundaries cannot overlap with coupled walls.

FMG initialization is not available.

The FAS multigrid scheme is not used.

Implicit residual smoothing cannot be enabled.

Overset meshing is not supported for incompressible flows in a closed domain.

The use of node weights for node-based gradients in postprocessing is not available for cases with overset

meshes.

.... Compatibilities

Overset meshing is compatible with the transient and steady-state solvers. Both laminar and turbulent

flow regimes with heat transfer are allowed as well as non-porous single phase flows, and Volume of

Fluid (VOF) and mixture multiphase flows. These applications are valid with overset for the listed

solver options and configurations. Unless otherwise specified, consider all other solver features and

models to be unsupported.

Supported Options and Models:

Pressure-based solver using:

– 2D (planar and axisymmetric) and 3D flows in the absolute velocity formulation

– Compressible flows

– Cell-based gradient methods: Green-Gauss Cell Based and Least Squares Cell Based

– All pressure interpolation schemes

– First-order and second-order spatial schemes

– Coupled scheme for pressure-velocity coupling

– Pseudo transient method

– First-order and (for stationary meshes only) second-order and bounded second-order transient formu-

lations

lations

Density-based solver using:

– All convective flux types (Roe-FDS, AUSM, and Low Diffusion Roe-FDS)

lations

turbulence models (Standard, RNG, and Realizable)

turbulence models (Standard, BSL, and SST)

Spalart-Allmaras turbulence model

Species transport model:

– single-phase flow only

– reactions must be disabled

VOF models:

– Open channel flow and surface gravity waves

– Cavitation and evaporation/condensation mass transfer

Mixture multiphase model:

– Non-granular flows

Cavitation and evaporation/condensation mass transfer in VOF/Mixture multiphase applications

Non-granular flows in multiphase applications

Dynamic and sliding meshes with the first-order transient formulation

User-defined scalars

User-defined functions (for information about overset-specific macros that can be useful when

writing user-defined functions, see Overset Mesh Looping Macros in the Fluent Customization

Manual)

All AMG options

All boundary conditions are supported with the following limitations:

– Non-interior face zone boundary conditions—exhaust fan, inlet vent, intake fan, outlet vent—are only

allowed on cell zones that are not participating in an overset interface

– Interior face zone boundary conditions—fan, porous-jump, and radiator—are only allowed on cell zones

that are not participating in an overset interface

Cell zone conditions

– Source terms may only be defined on cell zones not participating in an overset interface

– Fixed values may only be defined on cell zones not participating in an overset interface

– Multiple Reference Frame (MRF) model

Hybrid and standard initialization

An overset meshing solution may be obtained on any mesh type, including manually adapted meshes

Once you have read all of the related meshes into Fluent, use the following steps to setup an overset

. Change the boundary zones of component meshes to overset (boundary type), where needed.

Important

You must correctly specify the overset boundaries for all zones in an overset interface

before creating the overset interface. (Once overset interfaces are created you cannot

change any boundaries from overset to another type or from another type to overset.)

Setup → Boundary Conditions

<boundary> → Type → overset

. Create an overset interface between the cell zones that must be coupled. A case can have multiple inter-

faces. Each interface must have at least one background and one component mesh.

Domain → Interfaces → Overset

Figure . : Create/Edit Overset Interfaces Dialog Box

a.

Enter a name under Overset Interface.

a.

b. Select the zones of the interface in the Background Zones and Component Zones selection

lists. ANSYS Fluent allows you to create interfaces that contain only component zones; in such

cases, you do not select a background zone, but instead select two or more component zones.

c.

. (optional) Use the text user interface for additional control over the hole cutting step of the interface

initialization.

If certain boundary zones should not cut particular cell zones, use the define/overset-inter-

faces/cut-control/add text command to set up cut control.

If component meshes have no boundaries that will cut a cell zone, you can use the define/overset-

interfaces/cut-control/cut-seeds/cut-seeds-for-all-component-zones? text

command to ensure that all component zones get cut seeds (see Hole Cutting Control (p. )).

. (optional) Use the text user interface for additional control over the overlap minimization of the overset

interface. It can be helpful to revise the default settings if your overlapping meshes have uniform and

nearly identical resolutions or if local mesh distributions are irregular, as this may improve the computa-

tional efficiency and/or the solution quality. See Overlap Minimization (p. ) for details.

To specify whether the cell donor priorities used during minimization are based on the cell size or dis-

tance to the nearest boundary, use the following text command:

define → overset-interfaces → options → donor-priority-method

To revise the grid priorities during minimization, use the following text command.The grid priority for

each zone is an integer, and only the relative values between the zones matter.

define → overset-interfaces → grid-priorities

To disable overlap minimization entirely, use the following text command.This command is only

available globally and applies to all overset interfaces in the domain.

define → overset-interfaces → options → minimize-overlap?

Note that these steps only define an overset interface. Hole cutting occurs during solution initialization.

If a case contains overset face zones, but no defined overset interfaces, then Fluent creates a default

interface with the name default-overset-interface upon initialization. This default overset

interface contains all cell zones in the domain. If you know that some cell zones do not need to be

included in an overset interface, then you can increase the solution performance by manually creating

the interface and only including the relevant background and component meshes.

Fluent has several overset-specific postprocessing tools to help you analyze/understand the domain

connectivity. These tools are only available after the flow field is initialized and the domain connectivity

is established.

.... Overset Mesh Display

.... Overset Field Functions

.... Overset Cell Marks

.... Overset Interface listing

.... Overset Postprocessing Limitations

You can either visualize the complete mesh or just the active cells. If the Overset option is enabled

in the Mesh Display dialog box, by default only solve cells are shown. Disabling the Overset option

displays the complete surfaces.

Domain → Mesh → Display

You have the option to have receptor cells displayed along with the solve cells when Overset is se-

lected. You can enable this option via the TUI command define/overset-interfaces/op-

tions/render-receptor-cells?.

Note

When displaying contours of postprocessing quantities, dead cell values are never shown,

regardless of whether or not Overset is enabled in the Mesh Display dialog box.

There is an Overset Cell Type function available in the Cell Info... category in the Contours Dialog

Box (p. ). The integer function value depends on the overset cell type:

Integer Function Value

Cell Type

donor

solve

receptor

–

orphan

–

dead

This field function is also available in the Contours dialog box.

Results → Graphics → Contours → Edit...

.

Select Cell Info... and Overset Cell Type from the Contours of drop-down lists.

.

Choose the surfaces containing the overset cells you want to visualize and click Display.

Figure . : Contours of Overset Cell Type: Background Mesh

Figure . : Contours of Overset Cell Type: Component Mesh

Figure . : Contours of Overset Cell Type: Background Mesh (p. ) and Figure . : Contours of

Overset Cell Type: Component Mesh (p. ) display a background mesh and component mesh (se-

quentially) of Overset Cell Type for the cylinder problem shown in Figure . : Overset Component

and Background Mesh (p. ).

Note

If you want to display orphan cells, then you must enable the TUI command

define/overset-interfaces/options/render-receptor-cells?.

Note

If the expert options are enabled under define/overset-interfaces/options/expert,

then you can also choose to display Overset Donor Count and Overset Receptor Count under Cell

Info…. The Overset Donor Count is filled for each receptor and shows the number of donors. Similarly,

the Overset Receptor Count is filled for donor cells and shows the number of receptors that are

referencing the donors.

Note that the donor counts reported are the maximum number of donors available for the data interpol-

ation. The actual number of donors used by the solver may be less.

It can be difficult to interpret contours of overset cells in 3D. Often, it is more illustrative to mark a

certain type of overset cells and display these marked cells.

Using the text command define/overset-interfaces/mark-cells you can mark cells of

specified overset cell type (solve, receptor, donor, orphan, or dead), either globally or on a single cell

zone. This command automatically fills registers that can be displayed using the define/overset-

interfaces/display-cells text command.

Use the text command define/overset-interfaces/list to print overset interface related

information to the console. If the overset verbosity, define/overset-interfaces/op-

tions/verbosity, is set to , then counts of each overset cell type are printed per cell zone as

well.

Volume integrals are taken over all solve cells in the domain. This results in double counting where

solve cells overlap, leading to errors in volume integrals on overset meshes.

Similarly, surface integrals, including force and moment reports, will include errors when taken on

surfaces created for postprocessing (such as plane surfaces or rake surfaces) in regions where solve

cells or boundary zones overlap. If surface integrals are taken on boundary zones rather than created

surfaces and/or in a region without overlap, then the surface integrals are exact.

Important

Errors in integral evaluations scale with the size of the overlap.

When writing overset case files, it is recommended that you use the hierarchical data format (HDF),

as in this format the overset domain connectivity is saved in the case file. This makes it unnecessary

to reestablish the domain connectivity when reading an overset case into a new session. It also guar-

antees an identical connectivity when a case is read on a different number of compute nodes. For

more details about HDF, see Reading and Writing Files Using Hierarchical Data Format (HDF) (p. ).

When you write an overset case file in HDF and the case has not yet been initialized, ANSYS Fluent

will by default establish the domain connectivity prior to writing the file. This can be disabled using

the define/overset-interfaces/options/update-before-case-write? text command,

which is available after you enable the expert tools using the define/overset-interfaces/op-

tions/expert command.

The mesh checking capability in ANSYS Fluent examines various aspects of the mesh, including the

mesh topology, periodic boundaries, simplex counters, and (for axisymmetric cases) node position with

respect to the  axis, and provides a mesh check report with details about domain extents, statistics

related to cell volume and face area, and information about any problems associated with the mesh.

You can check the mesh by clicking the Check button in the General task page.

Setup →

General → Check

Important

It is generally a good idea to check your mesh right after reading it into Fluent, in order to

detect any mesh trouble before you get started with the problem setup.

The mesh check examines the topological information, beginning with the number of faces and nodes

per cell. A triangular cell (2D) should have  faces and  nodes, a tetrahedral cell (3D) should have

faces and  nodes, a quadrilateral cell (2D) should have  faces and  nodes, and a hexahedral cell (3D)

should have  faces and  nodes. Polyhedral cells (3D) will have an arbitrary number of faces and nodes.

Next, the face handedness and face node order for each zone is checked. The zones should contain all

right-handed faces, and all faces should have the correct node order.

The last topological verification is checking the element-type consistency. If a mesh does not contain

mixed elements (quadrilaterals and triangles or hexahedra and tetrahedra), ANSYS Fluent will determine

that it does not need to keep track of the element types. By doing so, it can eliminate some unnecessary

work.

For axisymmetric cases, the number of nodes below the  axis is listed. Nodes below the  axis are

work.

forbidden for axisymmetric cases, since the axisymmetric cell volumes are created by rotating the 2D

cell volume about the  axis; therefore nodes below the  axis would create negative volumes.

For solution domains with rotationally periodic boundaries, the minimum, maximum, average, and

prescribed periodic angles are computed. A common mistake is to specify the angle incorrectly. For

domains with translationally periodic boundaries, the boundary information is checked to ensure that

the boundaries are truly periodic.

Finally, the simplex counters are verified. The actual numbers of nodes, faces, and cells that Fluent has

constructed are compared to the values specified in the corresponding header declarations in the mesh

file. Any discrepancies are reported.

... Mesh Check Report

... Repairing Meshes

When you click the Check button in the General task page, a mesh check report will be displayed in

the console. The following is a sample of a successful output :

Mesh Check

Domain Extents:

x-coordinate: min (m) = -.000000e-, max (m) = .550000e-

y-coordinate: min (m) = .000000e+, max (m) = .500000e-

Volume statistics:

minimum volume (m3): .463287e-

maximum volume (m3): .508038e-

total volume (m3): .190433e-

minimum 2d volume (m3): .000589e-

maximum 2d volume (m3): .019523e-

Face area statistics:

minimum face area (m2): .199967e-

maximum face area (m2): .434403e-

Checking mesh.......................

Done.

The mesh check report begins by listing the domain extents. The domain extents include the minimum

and maximum ,

, and  coordinates in meters.

Done.

Then the volume statistics are provided, including the minimum, maximum, and total cell volume in

. A negative value for the minimum volume indicates that one or more cells have improper con-

nectivity. Cells with a negative volume can often be identified and viewed by creating an iso-value

field variable cell register (Field Variable (p. )). You can try adapting the mesh to resolve the negative

volume cells (Adapting the Mesh (p. )). You must eliminate these negative volumes before continuing

the flow solution process.

Next, the mesh report lists the face area statistics, including the minimum and maximum areas in

.

A value of  for the minimum face area indicates that one or more cells have degenerated. As with

negative volume cells, you must eliminate such faces. It is also recommended to correct cells that have

nonzero face areas, if the values are very small.

Besides the information about the domain extents and statistics, the mesh check report will also display

warnings based on the results of the checks previously described. You can specify that the mesh check

report displays more detailed information about the various checks and the mesh failures, by using

the following text command prior to performing the mesh check:

mesh → check-verbosity

You will then be prompted to enter the level of verbosity for the mesh check report. The possible

levels include:

This is the default level, and only notifies you that checks are being performed (for example,

Checking mesh...). The report will look like the previous example; while warnings will be displayed

below the domain extents and statistics, the names of the individual checks will not be listed as

they are conducted.

This level lists the individual checks as they are performed (for example, Checking right-handed

cells). Any warnings that result will be displayed immediately below the check that produced it.

This level provides the maximum information about the mesh check. The report will list the individual

checks as they are performed (for example, Checking right-handed cells); any warnings that result

will be displayed immediately below the check that produced it. Additional details about the check

failure will also be displayed, such as the location of the problem or the affected cells.

If the mesh check report indicates a mesh problem or if you receive warnings, you can investigate the

extent of the problem by printing the poor element statistics in the console. This can be accomplished

using the Report Poor Quality Elements button, located at the bottom of the Solution Methods

task page (Figure . : The Solution Methods Task Page (p. )). Note that this button is only available

when the mesh has poor quality elements. For more information about the Report Poor Quality Ele-

ments feature, see Robustness on Meshes of Poor Quality (p. ).

Figure . : The Solution Methods Task Page

Alternatively, you can print the poor element statistics via the following text command:

mesh → repair-improve → report-poor-elements

You can also visualize the invalid and poor elements by marking and displaying them by using the

Mesh... and Mark Poor Elements selections from the Field Value of drop-down lists of the Field

Variable Register dialog box (see Field Variable (p. ) for further details). Similarly, you can display

them using the Contours dialog box, by selecting Mesh... and Mark Poor Elements from the Contours

of drop-down lists. In either case, a value of  is assigned to the cells that are identified as invalid or

poor, as well as the cells that are adjacent to the face of an invalid or poor cell, and a value of  is as-

signed to all other cells.

The mesh check report will indicate if the mesh has problems that must be repaired, such as left-

handed faces and/or faces that have the wrong node order. If repairable failures are detected by the

mesh check, the Repair button in the Domain ribbon tab (Mesh group box) becomes available:

Domain → Mesh → Repair

Using the Repair button is the simplest way to attempt to correct your mesh problems. It will attempt

to correct a number of problems identified by the mesh check, including cells that have:

the wrong node order

the wrong face handedness or that are not convex

faces that are small or nonexistent

very poor quality (see Mesh Quality (p. ) for additional details)

Note that by default, the Repair button will only adjust the positions of interior nodes. If you want to

also modify the nodes on the boundaries of the mesh, use the following text command before you

repair the mesh:

mesh → repair-improve → allow-repair-at-boundaries

The Repair button may convert degenerate cells into polyhedra, based on skewness criteria (for more

information on how cells are converted, see Converting Skewed Cells to Polyhedra (p. )). If you want

to ensure that there are no polyhedra in the repaired mesh (for example, if you if plan on performing

hanging node adaption), you must disable such conversions using the following text command before

you repair the mesh:

mesh → repair-improve → include-local-polyhedra-conversion-in-repair

If you would like to only attempt to improve the poor quality cells, you can use the following text

command:

mesh → repair-improve → improve-quality

You can use the improve-quality text command multiple times, until the mesh is improved to

your satisfaction. For greater control over the degree to which the mesh is improved, you can perform

quality-based smoothing (as described in Smoothing (p. )).

It should be noted that both the Repair button and the improve-quality text command can be

CPU intensive, if there are a large number of poor quality cells in the mesh. If you are not as concerned

about cell quality, you can attempt to fix only the left-handed faces and faces with the wrong node

order. Begin by repairing the node order with the following text command:

mesh → repair-improve → repair-face-node-order

Because the left-handed faces may be a result of improper face node order, the previous text command

may resolve both issues at the same time. Be sure to perform another mesh check after entering the

repair-face-node-order command, to see if the mesh has been fully repaired.

If at any point the mesh check reveals that the mesh contains left-handed faces without any node order

issues, you can attempt to repair the face handedness by modifying the cell centroids with the following

mesh → repair-improve → repair-face-handedness

Once again, perform a mesh check to see if the text command was successful. The repair-face-

handedness text command is most effective for cells with high aspect ratios.

If the mesh check report includes a warning message such as

WARNING: node on face thread  has multiple shadows.

it indicates the existence of duplicate shadow nodes. This error occurs only in meshes with periodic-

type walls. You can repair such a mesh using the following text command:

mesh → repair-improve → repair-periodic

If the interface is rotationally periodic, you will be prompted for the rotation angle.

There are several methods for reporting information about the mesh after it has been read into ANSYS

Fluent. You can report the amount of memory used by the current problem, the mesh size, and statistics

about the mesh partitions. Zone-by-zone counts of cells and faces can also be reported.

Information about mesh statistics is provided in the following sections:

... Mesh Size

... Memory Usage

... Mesh Zone Information

... Partition Statistics

You can print out the numbers of nodes, faces, cells, and partitions in the mesh by clicking Info and

selecting Size, in the Domain ribbon tab (Mesh group box).

Domain → Mesh → Info → Size

A partition is a piece of a mesh that has been segregated for parallel processing (see Parallel Pro-

cessing (p. )).

A sample of the resulting output follows:

Mesh Size

Level     Cells       Faces       Nodes        Partitions

cell zones,  face zones.

If you are interested in how the cells and faces are divided among the different zones, click Info and

select Zones, in the Domain ribbon tab (Mesh group box), as described in Mesh Zone Informa-

tion (p. ).

If you are using the density-based coupled explicit solver, the mesh information will be printed for

each grid level. The grid levels result from creating coarse grid levels for the FAS multigrid convergence

Reporting Mesh Statistics

acceleration (see Full-Approximation Storage (FAS) Multigrid in the Theory Guide). A sample of the

resulting output is shown below:

Mesh Size

Level   Cells    Faces    Nodes     Partitions

During an ANSYS Fluent session you may want to check the amount of memory used and allocated

in the present analysis. ANSYS Fluent has a feature that will report the following information: the

numbers of nodes, faces, cells, edges, and object pointers (generic pointers for various mesh and

graphics utilities) that are used and allocated; the amount of array memory (scratch memory used for

surfaces) used and allocated; and the amount of memory used by the solver process.

You can obtain this information by clicking Info and selecting Memory Usage, in the Domain ribbon

tab (Mesh group box).

Domain → Mesh → Info → Memory Usage

The memory information will be different for Linux and Windows systems.

.... Linux Systems

On Linux systems, note the following definitions related to process memory information:

Process static memory is essentially the size of the code itself.

Process dynamic memory is the allocated heap memory used to store the mesh and solution variables.

Process total memory is the sum of static and dynamic memory.

....Windows Systems

On Windows systems, note the following definitions related to process memory information:

Process physical memory is the allocated heap memory currently resident in RAM.

Process virtual memory is the allocated heap memory currently swapped to the Windows system page

file.

Process total memory is the sum of physical and virtual memory.

The memory information does not include the static (code) memory.

Cortex runs in its own process, so the heap memory value includes storage for the mesh and solution

variables only.

On Windows systems, you can also get more information on the ANSYS Fluent process (or processes)

by using the Task Manager (see your Windows documentation for details). Examples of process image

names are as follows: cx1950.exe (Cortex), fl1950.exe (solver host), and fl_mpi1950.exe

(solver node).

You can print information in the console about the nodes, faces, and cells in each zone the by clicking

Info and selecting Zones, in the Domain ribbon tab (Mesh group box).

Domain → Mesh → Info → Zones

The mesh zone information includes the total number of nodes and, for each face and cell zone, the

number of faces or cells, the cell (and, in 3D, face) type (triangular, quadrilateral, and so on), the

boundary condition type, and the zone ID. Sample output is shown below:

Zone sizes on domain :

hexahedral cells, zone .

quadrilateral velocity-inlet faces, zone .

quadrilateral pressure-outlet faces, zone .

quadrilateral symmetry faces, zone .

quadrilateral interior faces, zone .

quadrilateral wall faces, zone .

nodes.

You can print mesh partition statistics in the console by clicking Info and selecting Partitions, in the

Domain ribbon tab (Mesh group box).

Domain → Mesh → Info → Partitions

The statistics include the numbers of cells, faces, interfaces, and neighbors of each partition. See Inter-

preting Partition Statistics (p. ) for further details, including sample output.

Since the ANSYS Fluent solver is face based, it supports polyhedral cells. The advantages that polyhedral

meshes have shown over some of the tetrahedral or hybrid meshes is the lower overall cell count, almost

times lower for unstructured meshes than the original cell count. Currently, there are three options

in ANSYS Fluent that allow you to convert your non-polyhedral cells to a polyhedra:

Converting the entire domain into polyhedral cells (applicable only for meshes that contain tetrahedral

and/or wedge cells).

Converting skewed tetrahedral cells to polyhedral cells.

Converting cells with hanging nodes/edges to polyhedral cells.

Information about polyhedral mesh conversion is provided in the following sections:

... Converting the Domain to a Polyhedra

... Converting Skewed Cells to Polyhedra

... Converting Cells with Hanging Nodes / Edges to Polyhedra

Converting the Mesh to a Polyhedral Mesh

Conversion of a mesh to polyhedra only applies to 3D meshes that contain tetrahedral and/or wedge

cells.

To begin the conversion process, ANSYS Fluent automatically decomposes each non-hexahedral cell

into multiple sub-volumes called “duals” (the shaded regions seen in the 2D example in Figure . : Con-

nection of Edge Centroids with Face Centroids (p. )). Each dual is associated with one of the original

nodes of the cell. These duals are then agglomerated into polyhedral cells around the original nodes.

Therefore, the collection of duals from all cells sharing a particular node makes up each polyhedral

cell (see Figure . : A Polyhedral Cell (p. )). The node that is now within the polyhedral cell is no

longer needed and is removed.

To better understand how duals are formed, you can consider the straightforward case of a tetrahedral

mesh. Each of the cells are decomposed in the following manner: first, new edges are created on each

face between the face centroid and the centroids of the edges of that face. Then, new faces are created

within the cell by connecting the cell centroid to the new edges on each face. These interior faces

establish the boundaries between the duals of a cell, and divide the cell into  sub-volumes. These

dividing faces may be adjusted and merged with neighboring faces during the agglomeration process,

in order to minimize the number of faces on the resultant polyhedral cell.

Note

By default, ANSYS Fluent checks the aspect ratio of boundary layer cells and if the aspect

ratios are high, ANSYS Fluent asks whether you want to preserve cells at the boundary layer

(which could be useful for keeping cell counts low when retaining boundary features). You

can override this default with the text command: mesh/polyhedra/options/pre-

serve-boundary-layer? (for additional information about these options, see mesh/

in the Fluent Text Command List).

Figure . : Connection of Edge Centroids with Face Centroids

Figure . : A Polyhedral Cell

Important

Hexahedral cells are not converted to polyhedra when the domain is converted, except

when they border non-hexahedral cells. When the neighboring cell is reconfigured as

polyhedra, the shared face of the hexahedral cell is decomposed into multiple faces as well,

resulting in a polyhedral cell. In such a case the shape of the original hexahedral cell is

preserved (that is the overall dimensions of the cell stay the same), but the converted cell

has more than the original  faces (see Figure . : A Converted Polyhedral Cell with Pre-

served Hexahedral Cell Shape (p. )).

Figure . : A Converted Polyhedral Cell with Preserved Hexahedral Cell Shape

Conversion proceeds in a slightly different manner in boundary layers that are modeled using thin

wedge cells. These cells are decomposed in the plane of the boundary surface, but not in the direction

normal to the surface. The resulting polyhedra will therefore preserve the thickness of the original

wedge cells (Figure . : Treatment of Wedge Boundary Layers (p. )). In most cases, the cell count

in the new polyhedral boundary layer will be lower than the original boundary layer.

Figure . : Treatment of Wedge Boundary Layers

To convert the entire domain of your mesh, click Make Polyhedra in the Domain ribbon tab (Mesh

group box).

Domain → Mesh → Make Polyhedra

The following is an example of the resulting message printed in the console:

Setup conversion to polyhedra.

Converting domain to polyhedra...

Creating polyhedra zones.

Processing face zones...........

Processing cell zones...

Building polyhedra mesh...................

Optimizing polyhedra mesh.....

>> Reordering domain using Reverse Cuthill-McKee method:

zones, cells, faces, done.

Bandwidth reduction = / = .

Done.

Figure . : The Original Tetrahedral Mesh (p. ), the original tetrahedral mesh of a section of a

manifold, is compared to Figure . : The Converted Polyhedral Mesh (p. ), which is the resulting

mesh after the entire domain is converted to a polyhedra.

Figure . : The Original Tetrahedral Mesh

Figure . : The Converted Polyhedral Mesh

Note that by default, the surfaces (that is, manifold zones of type interior) will be lost during the

conversion to polyhedra. If you would like to preserve any of these zones (in order to utilize them for

postprocessing, for example), use the following text command prior to the conversion:

mesh → polyhedra → options → preserve-interior-zones

You will be prompted to enter a string of characters, and only those interior surfaces with a name that

includes the string you specify will be preserved.

In parallel, a new partitioning will be stored after the conversion, but by default these new partitions

will not be made active (that is, migrated to the compute-nodes) as this requires significant additional

memory. The new partitions will be saved with the case file and used automatically when it is opened

in a new Fluent session; it is recommended that you then manually reorder the domain prior to calcu-

lating (using the mesh/reorder/reorder-domain text command). If you want to use the new

partitions in the current Fluent session, you should first ensure that no more than half of the available

memory of this system is currently used, and then you can manually migrate the partitions (using the

parallel/partition/use-stored-partitions text command) and reorder. If you know

prior to conversion that you will want to calculate a solution in the same session (and you have sufficient

memory), you can enable the following text command, so that the migration and reordering is performed

automatically as part of the conversion:

mesh → polyhedra → options → migrate-and-reorder?

Some limitations you will find with polyhedral meshes that you generally do not experience with

other cell types include:

Meshes that already contain polyhedral cells cannot be converted.

Meshes with hanging nodes/edges will not be converted.This includes meshes that have undergone

hanging node adaption (see Hanging Node Adaption in the Theory Guide), as well as CutCell meshes

(generated by Workbench or the meshing mode of Fluent, or resulting from the CutCell zone remeshing

method in the solution mode of Fluent) and hexcore meshes (generated when using the Hex Core

meshing scheme in GAMBIT or the Hexcore menu option in the meshing mode of Fluent).

The following mesh manipulation tools are not available for polyhedral meshes:

– the mesh/modify-zones/extrude-face-zone-delta text command

– the mesh/modify-zones/extrude-face-zone-para text command

– swapping

Meshes in which the domain has been converted to polyhedral cells are not eligible for adaption

with the default hanging node method, though they can be refined with the polyhedral unstructured

mesh adaption (PUMA) method. For more information about adaption, see Adapting the Mesh (p. ).

A mesh that is composed entirely of polyhedral cells has limitations when used in a dynamic mesh problem:

it cannot undergo dynamic layering, and the only remeshing method available is CutCell zone remeshing.

Smoothing is allowed for polyhedral cells, and diffusion-based smoothing is recommended over spring-

based smoothing (see Diffusion-Based Smoothing (p. ) for details).The linearly elastic solid smoothing

method is not compatible with polyhedral cells.

Since polyhedral meshes can have a much higher ratio of nodes to cells then tet or hex meshes, the use

of the node-based gradient method may result in a significant increase in memory consumption compared

with other gradient methods.

Another method of cell agglomeration is the skewness-based cluster approach. This type of conversion

is designed to convert only part of the domain. The objective is to convert only skewed tetrahedral

cells above a specified cell equivolume skewness threshold into polyhedra. By converting the highly

skewed tetrahedral cells, the quality of the mesh can be improved significantly.

A different algorithm is used for local conversion. This algorithm evaluates each highly skewed tetra-

hedral cell and all of the surrounding cells, to select an edge on the highly skewed cell that best

matches criteria for cell agglomeration. Then all of the cells that share this edge are combined into a

polyhedral cell. During the process, the data is interpolated from the original cells to the resultant

polyhedra.

There are certain limitations with this type of conversion:

– swapping will not affect polyhedral cells

The polyhedral cells that result from the conversion are not eligible for adaption with the default

hanging node method, though they can be refined with the polyhedral unstructured mesh adaption

(PUMA) method. For more information about adaption, see Adapting the Mesh (p. ).

Only tetrahedral cells are converted, as all other cells are skipped.

Meshes with hanging nodes / edges will not be converted.This includes meshes that have undergone

meshing scheme in GAMBIT or the Hexcore menu option in the meshing mode of Fluent). Note that if

the mesh is a CutCell / hexcore mesh in which the transitional cells have been converted to polyhedra,

then it does not have hanging nodes / edges and can therefore be converted.

face zone.

ANSYS Fluent provides a text command that allows you to convert cells that have hanging nodes /

edges into polyhedra. Such a conversion may be done in order to prevent errors associated with interior

walls (see Removing Hanging Nodes/Edges (p. )). Each of the converted polyhedra preserve the

shape of the original cell (that is, the overall dimensions of each cell stay the same), but the number

of faces associated with each cell increases (see Figure . : A Converted Polyhedral Cell with Preserved

Hexahedral Cell Shape (p. ) for an example). Such a conversion may be helpful for CutCell meshes

(generated by Workbench or the meshing mode of Fluent, or resulting from the CutCell zone

remeshing method in the solution mode of Fluent), as well as hexcore meshes (generated when using

the Hex Core meshing scheme in GAMBIT or the Hexcore menu option in the meshing mode of Fluent).

You could also convert the cells with hanging nodes in a mesh that has undergone hanging node

adaption (see Adapting the Mesh (p. )), but you would need to be sure that no further refine-

ment/coarsening of the mesh will be necessary.

To convert the cells with hanging nodes / edges, use the following text command:

mesh → polyhedra → convert-hanging-nodes

face zone.

There are several ways in which you can modify or manipulate the mesh after it has been read into

ANSYS Fluent. You can scale or translate the mesh, copy, merge, or separate zones, create or slit peri-

odic zones, fuse boundaries, and smooth and swap faces. Methods for partitioning meshes to be used

in a parallel solver are discussed in Mesh Partitioning and Load Balancing (p. ).

Important

Whenever you modify the mesh, you should be sure to save a new case file  (and a data

file, if data exists). If you have old data files that you would like to be able to read in again,

be sure to retain the original case file as well, as the data in the old data files may not cor-

respond to the new case file.

Information about mesh manipulation is provided in the following sections:

... Merging Zones

... Separating Zones

... Fusing Face Zones

... Creating Periodic Zones and Interfaces

... Slitting Periodic Zones

... Slitting Face Zones

... Orienting Face Zones

... Extruding Face Zones

... Replacing, Deleting, Deactivating, and Activating Zones

... Copying Cell Zones

... Replacing the Mesh

... Managing Adjacent Zones

... Reordering the Domain

... Scaling the Mesh

...Translating the Mesh

... Rotating the Mesh

... Improving the Mesh by Smoothing and Swapping

To simplify the solution process, you may want to merge zones. Merging zones involves combining

multiple zones of similar type into a single zone. Setting boundary conditions and postprocessing may

be easier after you have merged similar zones.

Zone merging is performed in the Merge Zones Dialog Box (p. ) (Figure . : The Merge Zones

Dialog Box (p. )).

Domain → Zones → Combine → Merge...

Figure . : The Merge Zones Dialog Box

....When to Merge Zones

ANSYS Fluent allows you to merge zones of similar type into a single zone. This is not necessary unless

the number of zones becomes prohibitive to efficient setup or postprocessing of the numerical ana-

lysis. For example, setting the same boundary condition parameters for a large number of zones can

be time-consuming and may introduce inconsistencies. In addition, the postprocessing of the data

often involves surfaces generated using the zones. A large number of zones often translates into a

large number of surfaces that must be selected for the various display options, such as color contouring.

Fortunately, surfaces can also be merged (see Grouping, Editing, Renaming, and Deleting Sur-

faces (p. )), minimizing the negative impact of a large number of zones on postprocessing efficiency.

Although merging zones can be helpful, there may be cases where you will want to retain a larger

number of zones. Since the merging process is not fully reversible, a larger number of zones provides

more flexibility in imposing boundary conditions. Although a large number of zones can make selection

Modifying the Mesh

of surfaces for display tedious, it can also provide more choices for rendering the mesh and the flow-

field solution. For instance, it can be difficult to render an internal flow-field solution. If the outer

domain is composed of several zones, the meshes of subsets of these zones can be plotted along

with the solution to provide the relationship between the geometry and solution field. Merging zones

may also adversely affect dynamic zones and mesh interfaces.

.... Using the Merge Zones Dialog Box

The procedure for merging multiple zones of the same type into a single zone is as follows:

. Select the zone type in the Multiple Types list.This list contains all the zone types for which there are

multiple zones.When you choose a type from this list, the corresponding zones will appear in the Zones

of Type list.

. Select two or more zones in the Zones of Type list.

. Click the Merge button to merge the selected zones. Note that if your case file has dynamic zones or

mesh interfaces, the Warning dialog box will open before the merge is initiated, allowing you to specify

whether you want to delete such zones or interfaces first (see Warning Dialog Box (p. ) for details).

Important

Remember to save a new case file (and a data file, if data exists).

Upon reading a mesh file, ANSYS Fluent automatically performs zone separations in two conditions. If

a face zone is attached to multiple cells zones in the preprocessor, the face zone will be separated so

that each one is attached to only one cell zone. Furthermore, if you have defined an internal face as

a wall type, an additional shadow wall zone will be generated (for example, for a wall named baffle,

a shadow wall zone named baffle-shadow will be generated).

There are several methods available in ANSYS Fluent that allow you to manually separate a single face

or cell zone into multiple zones of the same type. If your mesh contains a zone that you want to break

up into smaller portions, you can make use of these features. For example, if you created a single wall

zone when generating the mesh for a duct, but you want to specify different temperatures on specific

portions of the wall, you will need to break that wall zone into two or more wall zones. If you plan to

solve a problem using the sliding mesh model or multiple reference frames, but you forgot to create

different fluid zones for the regions moving at different speeds, you will need to separate the fluid

zone into two or more fluid zones.

Important

After performing any of these separations, you should save a new case file. If data exists, it is

automatically assigned to the proper zones when separation occurs, so you should also write

a new data file.The old data cannot be read on top of the case file in which the zones have

changed.

The maximum number of zones into which you can separate any one face zone or cell zone is

.

There are four ways to separate face zones and two ways to separate cell zones. The face separation

methods will be described first, followed by the cell separation tools. Slitting (decoupling) of periodic

zones is discussed in Slitting Periodic Zones (p. ).

Note that all of the separation methods allow you to report the result of the separation before you

commit to performing it.

.... Separating Face Zones

..... Methods for Separating Face Zones

..... Inputs for Separating Face Zones

For geometries with sharp corners, it is often easy to separate face zones based on significant angle.

Faces with normal vectors that differ by an angle greater than or equal to the specified significant

angle will be placed in different zones. For example, if your mesh consists of a cube, and all  sides

of the cube are in a single wall zone, you would specify a significant angle of °. Since the normal

vector for each cube side differs by ° from the normals of its adjacent sides, each of the  sides

will be placed in a different wall zone.

If you have a small face zone and would like to put each face in the zone into its own zone, you can

do so by separating the faces based on face. Each individual face (triangle, quad, or polygon) will

be separated into different zones.

You can also separate face zones based on cell registers. For example, you can mark cells based on

their location in the domain (region register), their boundary closeness (boundary register), field

values of some variable, or any of the cell marking methods discussed in Using Cell Registers (p. ).

When you specify which register is to be used for the separation of the face zone, all faces of cells

that are marked will be placed into a new face zone.

Finally, you can separate face zones based on contiguous regions. For example, when you use

coupled wall boundary conditions you need the faces on the zone to have a consistent orientation.

Consistent orientation can only be guaranteed on contiguous regions, so you may need to separate

face zones to allow proper boundary condition specification.

To break up a face zone based on angle, face, cell register mark, or region, use the Separate Face

Zones Dialog Box (p. ) (Figure . : The Separate Face Zones Dialog Box (p. )).

Domain → Zones → Separate → Faces...

Figure . : The Separate Face Zones Dialog Box

Important

If you are planning to separate face zones, you should do so before performing any ad-

aptions using the (default) hanging node adaption method. Face zones that contain

hanging nodes cannot be separated.

The steps for separating faces are as follows:

. Select the separation method (Angle, Face, Mark, or Region) under Options.

. Specify the face zone to be separated in the Zones list.

. If you are separating by face or region, skip to the next step. Otherwise, do one of the following:

If you are separating faces by angle, specify the significant angle in the Angle field.

If you are separating faces by mark, select the cell register to be used in the Registers list.

. (optional) To check what the result of the separation will be before you actually separate the face zone,

click the Report button.The report will look like the following example:

faces in contiguous region

Separates zone  into  zone(s).

. To separate the face zone, click the Separate button. A report will be printed in the console like the

following example:

Updating new zone information ...

created new zone wall-: from wall-

done.

Important

When you separate the face zone by cell register mark, you may sometimes find that a

face of a corner cell will be placed in the wrong face zone. You can usually correct this

problem by performing an additional separation, based on angle, to move the offending

face to a new zone. You can then merge this new zone with the zone in which you want

the face to be placed, as described in Merging Zones (p. ).

.... Separating Cell Zones

..... Methods for Separating Cell Zones

..... Inputs for Separating Cell Zones

If you have two or more enclosed cell regions sharing internal boundaries (as shown in Figure . : Cell

Zone Separation Based on Region (p. )), but all of the cells are contained in a single cell zone, you

can separate the cells into distinct zones using the separation-by-region method. Note that if the

shared internal boundary is of type interior, you must change it to another double-sided face zone

type (fan, radiator, and so on) prior to performing the separation.

Figure . : Cell Zone Separation Based on Region

You can also separate cell zones based on the marks stored in cell registers. You can mark cells using

any of the methods discussed in Using Cell Registers (p. ) (for example, you can mark cells with

a certain field value range or cells inside or outside a specified region). When you specify which re-

gister is to be used for the separation of the cell zone, cells that are marked will be placed into a

new cell zone.

To break up a cell zone based on region or cell register mark, use the Separate Cell Zones Dialog

Box (p. ) (Figure . : The Separate Cell Zones Dialog Box (p. )).

Domain → Zones → Separate → Cells...

Figure . : The Separate Cell Zones Dialog Box

Important

If you are planning to separate cell zones, you should do so before performing any adap-

tions using the (default) hanging node adaption method. Cell zones that contain hanging

nodes cannot be separated.

The steps for separating cells are as follows:

. Select the separation method (Mark or Region) under Options.

. Specify the cell zone to be separated in the Zones list.

. If you are separating cells by mark, select the cell register to be used in the Registers list.

. (optional) To check what the result of the separation will be before you actually separate the cell zone,

click the Report button.The report will look like this:

Separates zone  into two zones, with  and  cells.

. To separate the cell zone, click the Separate button. ANSYS Fluent will print the following information:

No faces marked on thread,

Separates zone  into two zones, with  and  faces.

All faces marked on thread,

Moved  cells from cell zone  to zone

created new zone interior-: from interior-

created new zone fluid-: from fluid-

done.

As shown in the example above, separation of a cell zone will often result in the separation of face

zones as well. When you separate by mark, faces of cells that are moved to a new zone will be placed

in a new face zone. When you separate by region, faces of cells that are moved to a new zone will

not necessarily be placed in a new face zone.

If you find that any faces are placed incorrectly, see the comment above, at the end of the inputs

for face zone separation.

The face-fusing utility is a convenient feature that can be used to fuse boundaries (and merge duplicate

nodes and faces) created by assembling multiple mesh regions. When the domain is divided into

subdomains and the mesh is generated separately for each subdomain, you will combine the subdo-

mains into a single file before reading the mesh into Fluent. For details, see Reading Multiple

Mesh/Case/Data Files (p. ). This situation could arise if you generate each block of a multiblock mesh

separately and save it to a separate mesh file. Another possible scenario is that you decided, during

mesh generation, to save the mesh for each part of a complicated geometry as a separate part file.

(Note that the mesh node locations need not be identical at the boundaries where two subdomains

meet; see Non-Conformal Meshes (p. ) for details.)

The Fuse Face Zones dialog box (Figure . : The Fuse Face Zones Dialog Box (p. )) allows you to

merge the duplicate nodes and delete these artificial internal boundaries.

Domain → Zones → Combine → Fuse...

Figure . : The Fuse Face Zones Dialog Box

The boundaries on which the duplicate nodes lie are assigned zone ID numbers (just like any other

boundary) when the mesh files are combined, as described in Reading Multiple Mesh/Case/Data

Files (p. ). You need to keep track of the zone ID numbers when tmerge or the meshing mode of

Fluent reports its progress or, after the complete mesh is read in, display all boundary mesh zones and

use the mouse-probe button to determine the zone names (see Controlling the Mouse Button Func-

tions (p. ) for information about the mouse button functions). Alternatively, you can specify a name

for the fused zone.

.... Inputs for Fusing Face Zones

The steps for fusing face zones are as follows:

. Select the zones to be fused in the Zones list.

Important

When using the Fuse Face Zone utility, each of the selected face zones must be fused

in its entirety with another face zone having the same connectivity. Partial fusing of

face zones is not supported.

. (Optional) If you would like to specify a name for the fused zone rather than use an automatically gener-

ated name (for instance, to preserve the original name of one of the face zones), disable Use default

name for new fused zone and enter the desired name.

. Click the Fuse button to fuse the selected zones.

If all of the appropriate faces do not get fused using the default Tolerance, you should increase it

and attempt to fuse the zones again. (This tolerance is the same as the matching tolerance discussed

in Creating Periodic Zones and Interfaces (p. ).) The Tolerance should not exceed ., or you may

fuse the wrong nodes.

You can also fuse zones using the mesh/modify-zones/fuse-face-zones text command, as

shown in the following example.

/mesh/modify-zones > fuse-face-zones

()

Zone to fuse() [()]  w1.top

Zone to fuse() [()]  w3

Zone to fuse() [()]  [Enter]

Choose from list (automatic w3 w1.top) or pick your own

Enter the fused zone name: [automatic]  w3

Name of zone  is changed into w3.

Fused list of zones successfully.

Important

Remember to save a new case file (and a data file, if data exists) after fusing faces.

..... Fusing Zones on Branch Cuts

Important

Meshes imported from structured mesh generators or solvers (such as FLUENT ) can often be O-

type or C-type meshes with a reentrant branch cut where coincident duplicate nodes lie on a peri-

odic boundary. Since ANSYS Fluent uses an unstructured mesh representation, there is no reason to

retain this artificial internal boundary. (You can preserve these periodic boundaries and the solution

algorithm will solve the problem with periodic boundary conditions.)

To fuse this periodic zone with itself, you must first slit the periodic zone, as described in Slitting

Periodic Zones (p. ). This will create two symmetry zones that you can fuse using the procedure

above.

Note that if you need to fuse portions of a non-periodic zone with itself, you must use the

mesh/modify-zones/fuse-face-zones text command.

mesh → modify-zones → fuse-face-zones

This command will prompt you for the name or ID of each zone to be fused. (You will enter the

same zone twice.) To change the node tolerance, use the mesh/modify-zones/matching-

tolerance text command.

ANSYS Fluent allows you to assign periodicity to your mesh by coupling a pair of face zones. If the

two zones are conformal (that is, have identical node and face distributions), then you can combine

them in a single boundary zone of type periodic. If the two zones are not identical at the boundaries

within a specified tolerance, then you can change them both to be of type interface and include them

in a non-conformal mesh interface that is periodic.

Important

Important

Remember to save a new case file (and a data file, if data exists) after creating or slitting a

periodic boundary.

To create a periodic boundary or interface, you can use the following text command.

mesh → modify-zones → create-periodic-interface

You can specify whether the face zones that make up the periodic pair are conformal or not, or let

Fluent automatically handle this decision (in which case a conformal pairing will be used if possible).

Next, you must specify the boundary zones, using either their full names or just their IDs; note that

the order in which you specify them is not significant. Then you must indicate if they are rotationally

or translationally periodic, and define the axis and offset. For pairings that are non-conformal (or could

potentially be, when using the automatic method), you must provide a name for the periodic mesh

interface that will / may be created. The following is an example this text command:

/mesh/modify-zones> create-periodic-interface

Periodic interface methods: auto, conformal, nonconformal

Enter method [auto]

Periodic zone [()]

Shadow zone [()]

Rotational periodic? (if no, translational) [yes]

Current axis origin is (  )

Enter a new axis origin? [no]

Current axis direction is (  )

Enter a new axis direction? [no]

Auto detect offset? [yes]

Create periodic zone? [yes]

Periodic interface name [] per-zone

Create matching interface? [no]

zone  deleted

Created conformal periodic interface.

When attempting to create a conformal periodic boundary, Fluent will check to see if the faces on the

selected zones “match” (that is, whether or not the nodes on corresponding faces are coincident). The

matching tolerance for a face is a fraction of the minimum edge length of the face. If the creation of

a conformal periodic boundary fails, you can change the matching tolerance using the following text

command. The tolerance should not exceed ., or you may match up the periodic zones incorrectly

and corrupt the mesh.

mesh → modify-zones → matching-tolerance

Note that when using the density-based solver, you can specify a pressure jump for a conformal peri-

odic zone; for details, see Periodic Flows (p. ).

For more information about non-conformal periodic boundaries and an alternate way to create them,

see Non-Conformal Meshes (p. ) and Using a Non-Conformal Mesh in ANSYS Fluent (p. ), respect-

ively.

If you want to decouple the zones in a periodic pair, you can use the mesh/modify-zones/slit-

periodic text command.

mesh → modify-zones → slit-periodic

You will specify the periodic zone’s name or ID, and Fluent will decouple the two zones in the pair

(the periodic zone and its shadow) and change them to two symmetry zones:

/mesh/modify-zones> slit-periodic

Periodic zone [()] periodic-

Slit periodic zone? [yes] yes

Slit periodic zone.

The face-zone slitting feature has two uses:

You can slit a single boundary zone of any double-sided type (that is, any boundary zone that has cells on

both sides of it) into two distinct zones.

You can slit a coupled wall zone into two distinct, uncoupled wall zones.

When you slit a face zone, Fluent will duplicate all faces and nodes, except those nodes that are located

at the ends (2D) or edges (3D) of the zone. One set of nodes and faces will belong to one of the res-

ulting boundary zones and the other set will belong to the other zone. The only ill effect of the shared

nodes at each end is that you may see some inaccuracies at those points when you graphically display

solution data with a slit boundary. (Note that if you adapt the boundary after slitting, you will not be

able to fuse the boundaries back together again.)

Before you can slit, you first need to select the zone in the Boundary Condition task page and change

the Type to wall. Upon changing the Type to wall, another shadow zone will be created (that is, if

the original zone is called rad-outlet, another zone called rad-outlet-shadow will be created). Then

you can apply the mesh/modify-zones/slit-face-zone text command on either of the walls

(that is, rad-outlet or rad-outlet-shadow) to separate them into two distinct walls.

Important

When a wall and wall-shadow pair is created by slitting a face zone, the wall will inherit the

zone id number and face orientation of the original zone. A new zone id number will be

created and assigned to the wall-shadow.

For example, the outlet of the radiator in an underhood application is typically of interior type (that

is, has cells on both sides). If you know the mass flow rate through this zone (either from other CFD

models or from test data) and want to apply it as a boundary condition at the radiator outlet, you first

need to slit the radiator outlet. To be able to slit it, select wall from the Type drop-down list in the

Boundary Conditions task page for this outlet. It will create a wall and a shadow. Then you can use

the TUI command (mesh/modify-zones/slit-face-zone) to slit them. After it is slit, two addi-

tional walls will be created, one facing one side of the outlet and another facing the other. Then you

can select the appropriate wall and change the Type to mass-flow-inlet and specify the mass flow

rate using the Mass-Flow Inlet Dialog Box (p. ). There is no option of mass-flow-inlet without first

slitting it.

Important

You should not confuse “slitting” a face zone with “separating” a face zone. When you slit

a face zone, additional faces and nodes are created and placed in a new zone. When you

separate a face zone, a new zone will be created, but no new faces or nodes are created;

the existing faces and nodes are simply redistributed among the zones.

.... Inputs for Slitting Face Zones

If you want to slit a face zone, you can use the mesh/modify-zones/slit-face-zone text

command.

mesh → modify-zones → slit-face-zone

You will specify the face zone’s name or ID, and Fluent will replace the zone with two zones:

/mesh/modify-zones > slit-face-zone

Face zone id/name [] wall-

face zone  created

Important

Remember to save a new case file (and a data file, if data exists) after slitting faces.

The faces of a boundary face zone (which have cells only on one side) are oriented such that the normals

are all pointing in one direction. However, for internal face zones (which have cells on both sides), the

normals are allowed to point in either direction. To orient them so that they all point in one direction,

you can use the following TUI command:

mesh → modify-zones → orient-face-zone

Having all of the normals oriented in one direction is needed for some boundary condition types. For

example, the fan boundary condition type determines the flow direction based on its normals. If some

of the normals are pointing in one direction and some in the other, the correct flow orientation cannot

be determined, which leads to incorrect results.

The ability to extrude a boundary face zone allows you to extend the solution domain without having

to exit Fluent. A typical application of the extrusion capability is to extend the solution domain when

recirculating flow is impinging on a flow outlet. The current extrusion capability creates prismatic or

hexahedral layers based on the shape of the face and normal vectors computed by averaging the face

normals to the face zone’s nodes. You can define the extrusion process by specifying a list of displace-

ments (in SI units) or by specifying a total distance (in SI units) and parametric coordinates.

Important

Note that extrusion is not possible from boundary face zones that have hanging nodes.

Extruding face zones is not allowed on polygonal face zones.

Extruding face zones is only allowed in the 3D version of ANSYS Fluent.

.... Specifying Extrusion by Displacement Distances

You can specify the extrusion by entering a list of displacement distances (in SI units) using the

mesh/modify-zones/extrude-face-zone-delta text command.

mesh → modify-zones → extrude-face-zone-delta

Note

This text command is not available in the parallel version of ANSYS Fluent.

You will be prompted for the boundary face zone ID or name and a list of displacement distances.

.... Specifying Extrusion by Parametric Coordinates

You can specify the extrusion by specifying a distance (in SI units) and parametric coordinates using

the mesh/modify-zones/extrude-face-zone-para text command.

mesh → modify-zones → extrude-face-zone-para

Note

You will be prompted for the boundary face zone ID or name, a total distance, and a list of parametric

coordinates. The list of parametric coordinates should begin with . and end with .. For example,

the following list of parametric coordinates would create two equally spaced extrusion layers: .,

., ..

ANSYS Fluent allows you to append or replace an existing cell zone in the mesh. You can also perman-

ently delete a cell zone and all associated face zones, or temporarily deactivate and activate zones

from your ANSYS Fluent case.

.... Replacing Zones

This feature allows you to replace a small region of a computational domain with a new region of

different mesh quality. This functionality will be required where you may want to make changes to

the geometry or mesh quality for any part of the domain. This ability of ANSYS Fluent will save you

time, since you can modify only the required part of the domain without remeshing the whole domain

every time.

The replacement mesh must be prepared in advance, with the following considerations:

The replacement mesh must contain a single cell zone.

The cell zone in the replacement mesh must be of the same zone type as the zone that is being replaced.

If the boundaries of the replacement mesh will form a non-conformal interface with existing zones (that

is, zones that are not replaced in the existing mesh), these boundaries should be based on the same

geometry as the existing zones. If there are sharp features (for example, -degree angles) or curvature

in the mesh, it is especially important that both sides of the interface closely follow that feature.

The replacement cell zone does not need to have the same name as the existing zone being replaced.

When naming the boundary zones of the replacement cell zone, note that boundary conditions will be

automatically transferred from the existing cell zone based on name. All boundaries of the replacement

cell zone that have unique names will be assigned the default boundary condition for that zone type.

Replacing a zone is performed using the Replace Cell Zone Dialog Box (p. ) (Figure . : The Replace

Cell Zone Dialog Box (p. )).

Domain → Zones → Replace Zone...

Figure . : The Replace Cell Zone Dialog Box

To replace a zone, do the following:

. Click Browse... and select the new or modified mesh containing the cell zone that will replace one of

the cell zones in the current mesh.

The name of the cell zone in the replacement mesh will be displayed in the Replace with list.

. Under Existing Zones, select the zone you want to replace.

. Under Replace with, select the zone from the replacement mesh.

. Enable/Disable Interpolate Data, if data already exists. If the replacement cell zone is geometrically

different, then Interpolate Data can be turned off to prevent data interpolation over the non-matching

geometries.

Important

Disable Interpolate Data if the zone being replaced is part of an overset interface.

. Click Replace to replace the selected zone.

. Set up the boundary conditions for any of the boundaries of the replacement mesh that do not share a

name with one of the existing boundaries.

.... Deleting Zones

To permanently delete zones, select them in the Delete Cell Zones Dialog Box (p. ) (Figure . : The

Delete Cell Zones Dialog Box (p. )), and click Delete.

Domain → Zones → Delete...

Figure . : The Delete Cell Zones Dialog Box

All of the cells, faces, and nodes associated with the cell zone will be deleted. If one of the faces is

of type interior and borders another cell zone, the face will automatically be changed to a wall and

will stay attached to the remaining cell zone.

.... Deactivating Zones

To deactivate zones, select them in the Deactivate Cell Zones Dialog Box (p. ) (Figure . : The

Deactivate Cell Zones Dialog Box (p. )), and click Deactivate.

Domain → Zones → Deactivate...

Figure . : The Deactivate Cell Zones Dialog Box

Deactivation will separate all relevant interior face zones (that is, fan, interior, porous-jump, or radiator)

into wall and wall-shadow pairs.

Note

When you deactivate a zone using the Deactivate Cell Zones dialog box, ANSYS Fluent will

remove the zone from the mesh and from all relevant solver loops.

Important

If a cell zone contains mesh interfaces it cannot be deactivated until the solution has been

initialized.

.... Activating Zones

You can reactivate the zones and recover the last data available for them using the Activate Cell

Zones Dialog Box (p. ) (Figure . : The Activate Cell Zones Dialog Box (p. )).

Domain → Zones → Activate...

Figure . : The Activate Cell Zones Dialog Box

Note

The Activate Cell Zones dialog box will only be populated with zones that were previously

deactivated.

After reactivation, you need to make sure that the boundary conditions for the wall and wall-shadow

pairs are restored correctly to what you assigned before deactivating the zones. If you plan to react-

ivate them at a later time, make sure that the face zones that are separated during deactivation are

not modified. Adaption, however, is supported.

You can create a copy of a cell zone that is offset from the original either by a translational distance

or a rotational angle. Note that in the copied zone, the bounding face zones are all converted to walls,

any existing cell data is initialized to a constant value, and non-conformal interfaces and dynamic

zones are not copied; otherwise, the model settings are the same as in the original zone.

To copy a zone, use the following text command:

mesh → modify-zones → copy-move-cell-zone

You will then be prompted to enter the ID of the zone you want to copy, and either the distance for

translation in each of the axes or the rotational angle, origin, and axis.

Note that if you want the copied zone to be connected to existing zones, you must either fuse the

boundaries (as described in Fusing Face Zones (p. )) or set up a non-conformal interface (as described

in Using a Non-Conformal Mesh in ANSYS Fluent (p. )).

ANSYS Fluent allows you to replace your mesh, so that you can continue to run your simulation on a

new mesh without having to manually copy the case file settings or interpolate the existing data. Re-

placing the mesh globally may be helpful, for example, if you would like to perform a mesh refinement

study with a prepared series of meshes, or if your results indicate that your current mesh is not of

sufficient quality. Note that the data interpolation is done automatically during the replacement if data

exists (that is, you have initialized the flow field or run a calculation).

Global mesh replacement is performed by clicking Replace Mesh... in the Domain ribbon tab Zones

group box), which opens the Select File dialog box (Figure . : The Select File Dialog Box (p. )).

.... Inputs for Replacing the Mesh

The steps for replacing the mesh using the Select File dialog box (Figure . : The Select File Dialog

Box (p. )) are as follows:

. Select the replacement mesh from the appropriate folder.

. By default, data is interpolated between matching zone pairs (that is, between the zones with the same

names in both the current mesh and the replacement mesh).You can enable the Interpolate Data

Across Zones option if you want to interpolate data across cell zones when replacing the mesh.This

option is appropriate when the matching zone pairs do not have the same interior zone boundaries.

Note that global conservation of data is not enforced when the Interpolate Data Across Zones option

is enabled, so it should only be used when absolutely necessary. For best data interpolation, the zone

boundaries of the replacement mesh should be coincident with those of the current mesh.

When running in parallel the replacement mesh gets partitioned such that matching cells reside

on the same compute node. In some cases, differences in mesh resolution can cause the mesh to

not be able to find its interpolation cell on the same compute node during interpolation. Fluent

then automatically enables Interpolate Data Across Zones to ensure successful data interpolation

across zones, even if you have not enabled the option. To avoid this behavior use the Scheme

command: (rpsetvar 'dynamesh/replace-mesh/partition-per-zone? #t). Note

that using this command comes at the expense of requiring additional repartitioning steps.

. Click the OK button to replace the mesh.

The following limitations apply when replacing meshes:

The boundary conditions of the zones in the current mesh are mapped onto the zones with the same

names in the replacement mesh, as described in Reading and Writing Boundary Conditions (p. ). If your

replacement mesh contains zones for which no match is found, these zones will have the default boundary

conditions for that zone type.

The replacement mesh is expected to be an ANSYS Fluent mesh (.msh) file.You can select an ANSYS

Fluent case (.cas) file instead, but be aware that only the mesh information will be used and all of the

setup information associated with that case file will be ignored.

If you intend to select an ANSYS Fluent case (.cas) file as the replacement mesh, you must first delete

any defined non-conformal mesh interfaces in the case file (as described in Using a Non-Conformal Mesh

in ANSYS Fluent (p. )).

You should ensure that the replacement mesh has the same mesh scaling as your current mesh.The data

interpolation will not work properly if the meshes are scaled differently.

In some cases you may want to identify and display the face zones which are adjacent to a cell zone.

You can do this using the Adjacency dialog box.

Domain → Zones → Adjacency...

Figure . : The Adjacency Dialog Box

Using the Adjacency dialog box (Figure . : The Adjacency Dialog Box (p. )) you can also optionally

rename zones based on their adjacency or with default names based on zone type. The steps to use

the Adjacency dialog box are:

. Open the Adjacency dialog box by clicking Adjacency... in the Domain ribbon tab (Zones group box).

. Select a zone under Cell Zone(s) to populate the Adjacent Face Zones list.You can use the 'Toggle Tree

View' icon (

) to group the cell zones by type. If the Multiple Cell Zones option is disabled, only one

cell zone can be selected at a time.

. Select the face zones you want to display in Adjacent Face Zones and click the Display Face Zones

button.

. Enable Draw Default Mesh to open the Mesh Display dialog box where you may choose to display mesh

zones.These will be displayed permanently while others will be displayed as currently selected in the

Adjacent Face Zones list.This is useful for finding your way through a new and complex mesh.

. Enable Rename Face Zones if you want to rename or clean up some of the names that may cause confu-

sion. See Renaming Zones Using the Adjacency Dialog Box (p. ) for more information.

.... Renaming Zones Using the Adjacency Dialog Box

You can rename selected zones from the Adjacency dialog box after enabling Rename Face Zones.

The following renaming methods are available:

Rename by Adjacency

appends the name of the cell zone to the type of the adjacent face zone. For example, if fluid is selected

in the Cell Zone(s) and interior is selected in the Adjacent Face Zones list, then renaming by adjacency

produces interior-fluid. If the name is already in use, the original zone ID is appended in addition in

order to create a unique name. Note that it is best if you avoid using long cell zone names.

Rename to Default

simply appends the original zone ID to the zone type. Enable Abbreviate Types to abbreviate the zone

type (for example, vi for velocity inlet, int for interior, ifc for interface, and so on).

Rename by Wildcard

performs pattern matching of the selected zone names against the pattern in the From text box (with

optional wildcards) and replaces a matching substring with the literal string in the To text box.Wildcard

characters * and ? are interpreted as follows:

A * at the beginning and/or end of the From pattern matches zero or more characters at the beginning

and/or end of the zone name that are retained during renaming with the rest of the name replaced

by the To string.

A * used anywhere except at the beginning or end of the From pattern is not supported and

may have unpredictable results.

A ? matches exactly one character and is considered part of the string to be replaced. Multiple ?

characters can be used to match substrings of more than one character.

For all of the renaming methods, you can enable Exclude Custom Names to exclude customized

names (those that do not conform to a recognized pattern or match any default names) from renaming.

This is a protective measure so as not to accidentally destroy your desired naming. Disabling this

option will unconditionally rename all selected zones according to the specified renaming method

and customized names will be permanently lost.

In a Fluent session that uses multiple processes, the mesh domain is automatically reordered when it

is read, in order to increase memory access efficiency. The reordering uses the Reverse Cuthill-McKee

algorithm  [] (p. ), and is applied to cells and faces.

A typical output produced during the domain reordering at read is shown below:

Building...

mesh

auto partitioning mesh by Metis (fast),

distributing mesh

parts...,

faces...,

nodes...,

cells...,

bandwidth reduction using Reverse Cuthill-McKee: / = .

The bandwidth is the maximum difference between neighboring cells in the zone—that is, if you

numbered each cell in the zone list sequentially and compared the differences between these indices.

Internally, ANSYS Fluent stores the computational mesh in meters, the SI unit of length. When mesh

information is read, it is assumed that the mesh was generated in units of meters. If your mesh was

created using a different unit of length (inches, feet, centimeters, and so on), you must scale the mesh

to meters. To do this, you can select from a list of common units to convert the mesh or you can

supply your own custom scale factors. Each node coordinate will be multiplied by the corresponding

scale factor.

Scaling can also be used to change the physical size of the mesh. For instance, you could stretch the

mesh in the  direction by assigning a scale factor of  in the  direction and  in the  and  directions.

This would double the extent of the mesh in the  direction. However, you should use anisotropic

scaling with caution, since it will change the aspect ratios of the cells in your mesh.

Important

If you plan to scale the mesh in any way, you should do so before you compute the view factors

(as part of an S2S radiation problem), initialize the flow, or begin calculations. Any data that

exists when you scale the mesh will be invalid.

It is a good practice to scale the mesh before setting up the case, especially when you plan to

create mesh interfaces or shell conduction zones.

Scaling the mesh makes the graphics window [Out of Date]. Right-click in the graphics window

and select Refresh Display to update the window.

You may have to click

to see the object in the graphics window after refreshing the dis-

play.

You will use the Scale Mesh Dialog Box (p. ) (Figure . : The Scale Mesh Dialog Box (p. )) to scale

the mesh from a standard unit of measurement or to apply custom scaling factors.

Setup →

General → Mesh → Scale...

Figure . : The Scale Mesh Dialog Box

.... Using the Scale Mesh Dialog Box

The procedure for scaling the mesh is as follows:

. Use the conversion factors provided by ANSYS Fluent by selecting Convert Units in the Scaling group

box.Then indicate the units used when creating the mesh by selecting the appropriate abbreviation for

meters, centimeters, millimeters, inches, or feet from the Mesh Was Created In drop-down list.The

Scaling Factors will automatically be set to the correct values (for example, . meters/inch).

If you created your mesh using units other than those in the Mesh Was Created In drop-down

list, you can select Specify Scaling Factors and enter values for X, Y, and Z manually in the

Scaling Factors group box (for example, the number of meters per yard).

. Click the Scale button.The Domain Extents will be updated to show the correct range in meters. If you

prefer to use your original unit of length during the ANSYS Fluent session, you can follow the procedure

described below to change the unit.

..... Changing the Unit of Length

As mentioned in Step . of the previous section, when you scale the mesh you do not change the

units; you just convert the original dimensions of your mesh points from your original units to meters

by multiplying each node coordinate by the specified Scaling Factors. If you want to work in your

original units, instead of in meters, you can make a selection from the View Length Unit In drop-

down list. This updates the Domain Extents to show the range in your original units and automat-

ically changes the length unit in the Set Units Dialog Box (p. ) (see Customizing Units (p. )).

Note that this unit will be used for all future inputs of length quantities.

..... Unscaling the Mesh

If you use the wrong scale factor, accidentally click the Scale button twice, or want to undo the

scaling for any other reason, you can click the Unscale button.“Unscaling” simply divides each of

the node coordinates by the specified Scale Factors. (Selecting m in the Mesh Was Created In list

and clicking on Scale will not unscale the mesh.)

..... Changing the Physical Size of the Mesh

You can also use the Scale Mesh Dialog Box (p. ) to change the physical size of the mesh. For

example, if your 2D mesh is  feet by  feet, and you want to model the same geometry with dimen-

sions twice as big ( feet by  feet), you can enter  for X and Y in the Scaling Factors group

box and click Scale. The Domain Extents will be updated to show the new range.

You can “move” the mesh by applying prescribed offsets to the Cartesian coordinates of all the nodes

in the mesh. This would be necessary for a rotating problem if the mesh were set up with the axis of

rotation not passing through the origin, or for an axisymmetric problem if the mesh were set up with

the axis of rotation not coinciding with the  axis. It is also useful if, for example, you want to move

the origin to a particular point on an object (such as the leading edge of a flat plate) to make an XY

plot have the desired distances on the  axis.

You can translate mesh points in ANSYS Fluent using the Translate Mesh Dialog Box (p. ) (Fig-

ure . : The Translate Mesh Dialog Box (p. )).

Domain → Mesh → Transform → Translate...

Figure . : The Translate Mesh Dialog Box

.... Using the Translate Mesh Dialog Box

The procedure for translating the mesh is as follows:

. Enter the desired translations in the ,

, and (for 3D)  directions (that is, the desired delta in the axes)

in the X, Y, and Z text-entry boxes in the Translation Offsets group box.You can specify positive or

negative real numbers in the current unit of length.

. Click the Translate button and redisplay the mesh.The Domain Extents will be updated to display the

new extents of the translated mesh. (Note that the Domain Extents are purely informational; you cannot

edit them manually.)

The ability to rotate the mesh is analogous to the ability to translate the mesh in ANSYS Fluent. You

can rotate the mesh about the ,

, or (for 3D)  axis and also specify the rotation origin. This option

is useful in the cases where the structural mesh and the CFD mesh are offset by a small angle.

You can rotate the mesh in ANSYS Fluent using the Rotate Mesh Dialog Box (p. ) (Figure . : The

Rotate Mesh Dialog Box (p. )).

Domain → Mesh → Transform → Rotate...

Figure . : The Rotate Mesh Dialog Box

.... Using the Rotate Mesh Dialog Box

The procedure for rotating the mesh is as follows:

. Specify the required Rotation Angle for the mesh.You can specify any positive or negative real number

in the correct unit of angle.

. In the Rotation Origin group box, enter X, Y, and (for 3D) Z coordinates to specify a new origin for the

axis of rotation.

. In the Rotation Axis group box, enter values for the X, Y, and (for 3D) Z axes to specify the vector for

the axis of rotation.

. Click the Rotate button and redisplay the mesh.

The Domain Extents will be updated to display the new extents of the rotated mesh. (Note that

the Domain Extents are purely informational; you cannot edit them manually.)

Smoothing and face swapping are tools that complement mesh adaption by increasing the quality of

the final numerical mesh. Smoothing repositions the nodes, and face swapping modifies the cell con-

nectivity to achieve these improvements in quality.

Important

Important

Only smoothing that is based on quality is recommended; face swapping and smoothing

based on skewness or a Laplacian operator have more limitations, and support for them

may be removed in a future release.

Important

Face swapping is applicable only to meshes with triangular or tetrahedral cells.

Important

Face swapping and smoothing based on skewness or a Laplacian operator are available

only for serial cases; only quality-based smoothing can be used for parallel cases.

.... Smoothing

.... Face Swapping

.... Combining Skewness-Based Smoothing and Face Swapping

The three smoothing methods that are available in ANSYS Fluent are:

quality-based smoothing

This method is the only recommended method, and is available for all types of meshes in serial

and parallel.

Laplacian smoothing

This method is not recommended, though it is available for all types of meshes in serial (and is

best suited for quadrilateral and hexahedral meshes).

skewness-based smoothing

This method is not recommended, though it is available for triangular and tetrahedral meshes in

serial; it can be used alternatively with face swapping (see Combining Skewness-Based Smoothing

and Face Swapping (p. )).

..... Quality-Based Smoothing

Smoothing that is based on quality is performed using the Improve Mesh Dialog Box (p. ) (Fig-

ure . : The Improve Mesh Dialog Box (p. )).

Domain → Mesh → Quality → Improve Mesh Quality...

Figure . : The Improve Mesh Dialog Box

ANSYS Fluent divides the mesh into a number of “bins”, each of which contain a certain number of

cells. Improvements are attempted on the cells in those bins that exhibit the lowest orthogonal

quality (as defined in Mesh Quality (p. )). As part of this method, you specify the percentage of

the total number of cells, in order to determine how many bins are modified.

Note that this smoothing is similar to when you use the mesh/repair-improve/improve text

command. The advantage of using the Improve Mesh dialog box rather than the text command is

that you can control the percentage of the cells that ANSYS Fluent attempts to improve.

To perform quality-based smoothing, do the following steps:

. In the Improve Mesh Dialog Box (p. ) (Figure . :The Improve Mesh Dialog Box (p. )), enter the

Percentage of Cells to be Improved.

Important

Quality-based smoothing will be CPU intensive if you specify a large value for the

Percentage of Cells to be Improved. It is recommended that you enter a small value

initially, and then perform the smoothing process multiple times, if necessary. Note

that the maximum percentage allowed is %.

. Specify the number of successive smoothing sweeps to be performed on the mesh in the Number of

Iterations number-entry box.The default value is .

. Click the Improve button.

..... Laplacian Smoothing

When you use this method, a Laplacian smoothing operator is applied to the unstructured mesh to

reposition nodes. The new node position is the average of the positions of its node neighbors. The

computed node position increment is multiplied by the relaxation factor (which is set to a value

between . and . ). A value of zero for the relaxation factor results in no movement of the node,

and a value of unity results in movement equivalent to the entire computed increment. Figure . : Res-

ult of Smoothing Operator on Node Position (p. ) illustrates the new node position for a typical

configuration of quadrilateral cells. The dashed line is the original mesh and the solid line is the final

mesh.

Figure . : Result of Smoothing Operator on Node Position

This repositioning strategy improves the skewness of the mesh, but relaxes the clustering of node

points. In extreme circumstances, the present operator may create mesh lines that cross over the

boundary, creating negative cell volumes. This is most likely to occur near sharp or coarsely resolved

convex corners, especially if you perform multiple smoothing operations with a large relaxation

factor. Figure . : Initial Mesh Before Smoothing Operation (p. ) illustrates an initial tetrahedral

mesh before one unrelaxed smoothing iteration creates mesh lines that cross over each other (Fig-

ure . : Mesh Smoothing Causing Mesh-Line Crossing (p. )).

Figure . : Initial Mesh Before Smoothing Operation

Figure . : Mesh Smoothing Causing Mesh-Line Crossing

The default smoothing parameters are designed to improve mesh quality with minimal adverse effects,

but it is recommended that you save a case file before smoothing the mesh. If you apply a conser-

vative relaxation factor and start with a good quality initial mesh, the frequency of failure due to

smoothing is extremely low in two dimensions. However, corruption of the mesh topology occurs

much more frequently in three dimensions, particularly with tetrahedral meshes.

The smoothing operator can also be applied repeatedly, but as the number of smoothing sweeps

increase, the node points have a tendency to pull away from boundaries and the mesh tends to lose

To perform Laplacian smoothing, enter the mesh/smooth-mesh text command in the console and

respond to the prompts as follows:

. Enter "laplace" for the type of smoothing.

. Specify the number of successive smoothing sweeps to be performed on the mesh in response to the

number of iterations prompt.The default value is .

. Specify the factor by which to multiply the computed position increment for the node in response to

the relaxation factor prompt.The lower the factor, the more reduction in node movement.

..... Skewness-Based Smoothing

When you use skewness-based smoothing, ANSYS Fluent applies a smoothing operator to the mesh,

repositioning interior nodes to lower the maximum skewness of the mesh. ANSYS Fluent will try to

move interior nodes to improve the skewness of cells with skewness greater than the specified

“skewness threshold”. This process can be very time consuming, so perform smoothing only on cells

with high skewness.

Improved results can be obtained by smoothing the nodes several times. There are internal checks

that will prevent a node from being moved if moving it causes the maximum skewness to increase,

but it is common for the skewness of some cells to increase when a cell with a higher skewness is

being improved. Thus, you may see the average skewness increase while the maximum skewness

is decreasing.

Important

Carefully consider whether the improvements to the mesh due to a decrease in the

maximum skewness are worth the potential increase in the average skewness. Performing

smoothing only on cells with very high skewness (for example, . or .) may reduce

the adverse effects on the average skewness.

To perform skewness-based smoothing, enter the mesh/smooth-mesh text command in the

console and respond to the prompts as follows:

. Enter "skewness" for the type of smoothing.

. Specify the minimum cell skewness value for which node smoothing will be attempted in response to

the skewness threshold prompt. ANSYS Fluent will try to move interior nodes to improve the

skewness of cells with skewness greater than this value. By default, skewness threshold is set to . for

2D cases and . for 3D cases.

While it is not recommended over smoothing (and support for it may be removed in future releases),

face swapping can be used to improve the quality of a triangular or tetrahedral mesh in the serial

version of ANSYS Fluent.

To perform face swapping, enter the mesh/swap-mesh-faces text command repeatedly until the

console report declares that  faces were swapped out. The console report will display the total

number of faces that were visited and tested for possible face swapping.

.....Triangular Meshes

The approach for triangular meshes is to use the Delaunay circle test to decide if a face shared by

two triangular cells should be swapped. A pair of cells sharing a face satisfies the circle test if the

circumcircle of one cell does not contain the unshared node of the second cell. Figure . : Examples

of Cell Configurations in the Circle Test (p. ) illustrates cell neighbors in the circle test. In cases

where the circle test is not satisfied, the diagonal or face is swapped, as illustrated in Fig-

ure . : Swapped Faces to Satisfy the Delaunay Circle Test (p. ).

Figure . : Examples of Cell Configurations in the Circle Test

Figure . : Swapped Faces to Satisfy the Delaunay Circle Test

Repeated application of the face-swapping technique will produce a constrained Delaunay mesh. If

you have a Delaunay mesh, it is a unique triangulation that maximizes the minimum angles in the

mesh. Thus, the triangulation tends toward equilateral cells, providing the most equilateral mesh

for the given node distribution. For more information on Delaunay mesh generation, see Generating

Tetrahedral Meshes (p. ) in the Fluent Meshing section of the User’s Guide.

.....Tetrahedral Meshes

For tetrahedral meshes, face swapping consists of searching for configurations of three cells sharing

an edge and converting them into two cells sharing a face to decrease skewness and the cell count

(see Figure . : 3D Face Swapping (p. )).

Figure . : 3D Face Swapping

As mentioned in Skewness-Based Smoothing (p. ), skewness-based smoothing should usually be

alternated with face swapping. Guidelines for this procedure are presented here.

Perform four smoothing iterations using a skewness threshold of . for 3D cases, or . for 2D

cases.

Swap until the number of faces swapped decreases to .

For 3D meshes, decrease the skewness threshold to . and repeat the smoothing/swapping pro-

cedure.

Chapter : Cell Zone and Boundary Conditions

This chapter describes the cell zone and boundary condition options available in ANSYS Fluent. Details

regarding the cell zone and boundary condition inputs and the internal treatment at boundaries are

provided.

The information in this chapter is divided into the following sections:

.. Overview

.. Cell Zone Conditions

.. Boundary Conditions

.. Editing Multiple Boundary Conditions at Once

.. Boundary Acoustic Wave Models

.. User-Defined Fan Model

.. Profiles

.. Coupling Boundary Conditions with GT-POWER

.. Coupling Boundary Conditions with WAVE

Cell zone and boundary conditions specify the flow and thermal variables on the boundaries of your

physical model. They are, therefore, a critical component of your ANSYS Fluent simulations and it is

important that they are specified appropriately.

In this chapter, most of the cell zones and boundary conditions will be described in detail, and an ex-

planation of how to set them and where they are most appropriately used will be provided.

... Available Cell Zone and Boundary Types

...The Cell Zone and Boundary Conditions Task Pages

... Changing Cell and Boundary Zone Types

... Setting Cell Zone and Boundary Conditions

... Copying Cell Zone and Boundary Conditions

... Changing Cell or Boundary Zone Names

... Defining Non-Uniform Cell Zone and Boundary Conditions

... Defining and Viewing Parameters

... Selecting Cell or Boundary Zones in the Graphics Display

... Operating and Periodic Conditions

... Highlighting Selected Boundary Zones

... Saving and Reusing Cell Zone and Boundary Conditions

The cell zone and boundary zone types available in ANSYS Fluent are classified as follows:

Table . : Zone Types by Category

Zone Types

Category

axis, degassing, exhaust fan, inlet vent, intake fan, interface, mass-flow

inlet, mass-flow outlet, outflow, outlet vent, overset, pressure far-field,

External

pressure inlet, pressure outlet, symmetry, velocity inlet, and wall (one-sided

only)

fan, interior, porous jump, radiator, RANS/LES interface, and wall (two-sided

only)

Internal

periodic

Periodic

fluid, solid (porous media and 3D fans are a type of fluid cell)

Cells

Note that internal boundary zones are connected with the cells on both of their faces, whereas external

boundary zones are connected with the cells on only one of their faces.

The Cell Zone Conditions and Boundary Conditions task pages (Figure . : The Boundary Conditions

Task Page (p. )) display lists of the zones (which can be grouped by name or zone type), and allow

you to revise their settings and perform other related actions. They provide an alternate setup method

to working directly in the Outline View tree.

Setup →

Cell Zone Conditions

Setup →

Cell Zone and Boundary Conditions

Figure . : The Boundary Conditions Task Page

The sections that follow explain how to perform operations, mostly using the Outline View tree, however

these same operations can also be completed using the Cell Zone Conditions or Boundary Conditions

task page. The sections also explain how to use the mouse and the graphics display in conjunction

with the dialog box.

Note — You can modify individual boundary conditions and cell zones by expanding the Cell Zones

and Boundary Conditions branches in the tree, and right-clicking the boundary condition or cell zone

you want to modify.

Before you set any cell zone or boundary conditions, you should check the zone types of all boundary

zones and change any if necessary. For example, if your mesh includes a pressure inlet, but you want

to use a velocity inlet instead, you will need to change the pressure-inlet zone to a velocity-inlet zone.

Note that external and internal boundary zones (as listed in Table . : Zone Types by Category (p. ))

can only be changed to a zone of the same category.

The steps for changing a zone type using the graphical user interface are as follows:

. Select the boundary or cell zone in the tree (under Setup/Boundary Conditions or Setup/Cell Zone

Conditions). Note that you can select multiple zones by holding the Shift or Ctrl keys when selecting,

though you must ensure that all of the selections are of the same category.

. Right-click a selected boundary or cell zone, and select the correct zone type from the Type sub-menu.

Overview

You can also change the zone type using either the define/boundary-conditions/zone-type

or the define/boundary-conditions/modify-zones/zone-type text command. To change

the type for multiple zones of the same category through a single action, you can enter a list of names

or IDs contained within a pair of parentheses at the prompt, as shown in the following example (which

changes zone  and  to be pressure inlets):

> define/boundary-conditions/zone-type

zone id/name/list [] ( )

external-type> pressure-inlet

When changing the cell or boundary zone type, note the following:

For zones that have the default name (that is, <type> - <ID>), the name will be changed automatically

along with the type.

When you have a large number of internal boundary zones that you want to change to or from a wall /

shadow pair, it is recommended that you change their type with a single action (either by multi-selecting

in the tree or by using parentheses at the text command prompt); this will greatly reduce the processing

time associated with the change.

When changing a wall / shadow pair to one of the other internal types (fan, interior, porous jump, radiator,

or RANS/LES interface), you can select either the wall or the wall-shadow to change. In either case, the

resulting zone will retain the ID and orientation of the wall zone and the wall-shadow zone will be deleted.

Note that you cannot use this method to change zone types to or from the periodic type, since additional

restrictions exist for this boundary type. Creating Periodic Zones and Interfaces (p. ) explains how to

create and uncouple periodic zones.

If you are using one of the general multiphase models (VOF, mixture, or Eulerian), the procedure for changing

types is slightly different. See Steps for Setting Boundary Conditions (p. ) for details.

In ANSYS Fluent, boundary conditions are associated with zones, not with individual faces or cells. If

you want to combine two or more zones that will have the same boundary conditions, see Merging

Zones (p. ) for information about merging zones.

To set cell zone and boundary conditions for a particular zone, perform one of the following sequences:

. Right-click the name of zone in the tree (under Setup/Boundary Conditions or Setup/Cell Zone Condi-

tions).

. Select Edit....

Note

You can group Boundary Conditions based on adjacency, allowing you to see which

boundaries belong to the same cell zone. To do this, right-click the Boundary Conditions

branch in the Outline View tree and select Group By/Adjacency.

Group By → Adjacency

or

. Select the zone from the Zone list in the Cell Zone Conditions or Boundary Conditions task page.

. Click the Edit... button.

Overview

The dialog box for the selected cell or boundary zone will open, and you can specify the appropriate

Important

Overview

Important

If you are using one of the general multiphase models (VOF, mixture, or Eulerian), the pro-

cedure for setting conditions is slightly different from that described above. See Steps for

Setting Boundary Conditions (p. ) for details.

You can use the text command: define/boundary-conditions/set/ to define one or more

settings at a single or multiple boundaries/cell zones of a given type. This facilitates quick and efficient

setup of cell/boundary conditions for cases with large numbers of zones.

To edit multiple boundaries you can either provide a list of boundary names / IDs enclosed in paren-

thesis:

/define/boundary-conditions/set> wall

(rotor-hub rotor-shroud rotor-blade- rotor-blade- stator-hub stator-shroud stator-blade- stator-blade-)

zone(s) to set boundary conditions() [rotor-hub] (rotor-blade- rotor-blade-)

or you can use a wildcard pattern for the boundary names:

zone(s) to set boundary conditions() [rotor-hub] (rotor-blade-*)

For additional information on formatting lists in the console, see Lists.

After entering the zone(s) you want to change you will be prompted for what setting to change.

Pressing Enter will list the available settings.

When you have changed all of the desired settings, press q to exit the define/boundary-condi-

tions/set/<type> command. Note that some settings will not take effect until after you have

exited the command, by pressing q.

You can copy cell zones and boundary conditions from one zone to other zones of the same type. If,

for example, you have several wall zones in your model and they all have the same boundary conditions,

you can set the conditions for one wall, and then simply copy them to the others.

The procedure for copying cell zone or boundary conditions is as follows:

. Right-click the name of zone in the tree that you want to copy (under Setup/Boundary Conditions or

Setup/Cell Zone Conditions) and select Copy....This will open the Copy Conditions dialog box (Fig-

ure . :The Copy Conditions Dialog Box (p. )).

Figure . : The Copy Conditions Dialog Box

. In the From Cell Zone or From Boundary Zone list, confirm that the zone that has the conditions you

want to copy is selected.

. In the To Cell Zones or To Boundary Zones list, select the zone or zones to which you want to copy the

. Click Copy. ANSYS Fluent will set all of the cell zones or boundary conditions for the zones selected in

the To Cell Zones or To Boundary Zones list to be the same as the conditions for the zone selected in

the From Cell Zone or From Boundary Zone list. (You cannot copy a subset of the conditions, such as

only the thermal conditions.)

Note that you cannot copy conditions from external walls to internal (that is, two-sided) walls, or vice

versa, if the energy equation is being solved, since the thermal conditions for external and internal

walls are different.

Important

Important

cedure for copying boundary conditions is slightly different. See Steps for Copying Cell

Zone and Boundary Conditions (p. ) for details.

The default name for a zone is <type> - <ID> (for example, pressure-inlet-). In some cases, you may

want to assign more descriptive names to the boundary zones. If you have two pressure-inlet zones,

for example, you might want to rename them small-inlet and large-inlet. (Changing the name of a

zone will not change its type. Instructions for changing a zone’s type are provided in Changing Cell

and Boundary Zone Types (p. ).)

You can rename boundaries and cell zones directly within the tree, by selecting the zone that you

want to rename, then clicking the name (slow double-click).

Overview

Alternatively, you can rename a zone by following these steps:

tions).

. Select Edit... to open the dialog box for the selected zone.

. Enter a new name under Zone Name.

. Click the OK button.

Note

If you specify a non-default name for a zone and then change its type, the name you specified

will be retained; the automatic name change that accompanies a change in type occurs

only for those with the default name.

Most conditions at each type of boundary zone can be defined as profile functions instead of constant

values. You can use a profile contained in an externally generated profile file, or a function that you

create using a user-defined function (UDF). Profiles are described in Profiles (p. ), and user-defined

functions are described in the separate Fluent Customization Manual.

You can define a series of cases based on a set of parametric values. These parameters may be defined

for numeric cell zone and boundary condition settings. This is especially useful if you are using Work-

bench and performing parametric studies (optimization), comparing cases with different boundary

settings; information about such usage can be found in see Working with Parameters and Design

Points in the Workbench User's Guide. If you are not running ANSYS Fluent through Workbench, then

you can use the parameter settings to define the same boundary condition value to different bound-

aries having the same units, or to use the Adjoint-Based Optimizer to optimize a geometry for multiple

objectives at multiple operating conditions (see Using the Gradient-Based Optimizer (p. )).

Note

For more information about using parameters with ANSYS Fluent in ANSYS Workbench, see

Working With Input and Output Parameters in Workbench in the separate Fluent in Work-

bench User's Guide.

The parameters that you have defined in the various boundary condition dialog boxes are accessed

by clicking the Parameters... button in the Cell Zone Conditions or Boundary Conditions task page.

The Parameters dialog box will open, as shown in Figure . : The Parameters Dialog Box (p. ), listing

all of the input parameters that you have created in the various boundary condition dialog boxes.

Figure . : The Parameters Dialog Box

In the Parameters dialog box, under the Input Parameters list, you can

Edit the input properties using the Parameter Expression dialog box, which is the same dialog box used

to create parameters.This dialog box can also be accessed by selecting New Input Parameter... from the

drop-down lists in the boundary conditions dialog boxes, as described later in this section.

Important

If you are using ANSYS Fluent in ANSYS Workbench, you cannot edit the input parameters,

you can only view them. For more information, see the separate ANSYS Fluent in ANSYS

Workbench User's Guide.

Delete input parameters that are not assigned to a setting.

More options exist under the More drop-down list (see Working With Advanced Parameter Options (p. )):

Overview

Use in Scheme Procedure

displays the Use Input Parameter in Scheme Procedure Dialog Box (p. ) where you can apply an input

parameter using a Scheme procedure.

Use in UDF

displays the Use Input Parameter for UDF Dialog Box (p. ) where you can make an input parameter

available in a user-defined function.

In the Parameters dialog box, under the Output Parameters list, you can also

Create output parameters.These are single values generated by existing reports or monitors.You can

generate the output parameters for Fluxes, Forces, Surface, Volume, Drag, Lift, Moments, and User

Defined report definitions.These output parameters are discussed in greater detail in Creating Output

Parameters (p. ).

Edit existing output parameters.

More options exist under the More drop-down list:

Delete

removes the selected output parameter from the list of Output Parameters.

Rename

Delete

Rename

allows you to edit the name of the output parameter through the Rename dialog box.

Print to Console

will output values to the console window. If you select multiple output parameters, then the output

includes values from multiple output parameters.

Print All to Console

outputs the values from all output parameters to the console window.

Write...

allows you to store the output to a file. A dialog box is displayed allowing you to provide a file name.

Write All...

prompts you for a file name and then writes the values for all of the output parameters to a file.

Important

Changing the units for a quantity changes the value for any input parameter using that

quantity.

Note

Various ANSYS Fluent setup-related input quantities (of type real and profile) can be assigned

to an input parameter (indicated by the New Input Parameter... option in the corresponding

drop-down list or menu next to the field). Clicking this option opens the Figure . : The

Parameter Expression Dialog Box (p. ) where you can create the input parameter.

.... Creating a New Parameter

You can create a new cell zone or boundary condition parameter, as shown in Figure . : The New

Input Parameter/Expression... Selection (p. ).

Figure . : The New Input Parameter/Expression... Selection

When you select New Input Parameter/Expression... from the drop-down list, the Parameter Ex-

pression dialog box (Figure . : The Parameter Expression Dialog Box (p. )) will open where you

will

Enter the Name of the parameter expression.

Specify the Definition as a constant.

will

The Used In field displays information about where the parameter is utilized. Note that this field will be

populated after you create an input parameter.

Overview

Figure . : The Parameter Expression Dialog Box

Once the parameter is defined in the Parameter Expression dialog box, the name of the parameter

will appear in the drop-down list of the property you are defining, as seen in Figure . : The New Input

Parameter/Expression... Selection (p. ).

Important

Input parameter expressions must be directly defined as a constant value including appro-

priate units; it may not reference another expression.

Note

ANSYS Fluent automatically creates generic default names for new input and output

parameters (for example, parameter_1, parameter_2, parameter_3, and so on) If

a parameter is deleted, the default name is not reused. For example, if you have paramet-

er_1, parameter_2, and parameter_3, then delete parameter_2 and create a new

parameter, the default name for the new parameter will be parameter_4.

....Working With Advanced Parameter Options

Various ANSYS Fluent setup related input quantities can be assigned to an input parameter. You can

define a series of simulations based on a set of parametric values that are managed both in ANSYS

Fluent and in Workbench. These parameters may be defined for numeric cell zone and boundary

condition settings using the New Input Parameter… option in the corresponding drop-down list or

menu adjacent to a specific input setting. However, various ANSYS Fluent settings are not supported

by these methods.

You can mitigate this limitation using input parameters through Scheme procedures and user-defined

functions (UDFs), and define input parameters for various ANSYS Fluent simulation related settings.

..... Defining Scheme Procedures With Input Parameters

..... Defining UDFs With Input Parameters

..... Using the Text User Interface to Define UDFs and Scheme Procedures With Input Parameters

To use a Scheme procedure with input parameters, in the Parameters dialog box under Input

Parameters, select More, then choose Use in Scheme Procedure to display the Use Input Parameter

in Scheme Procedure Dialog Box (p. ) where you can register the input parameters that can be

used in Scheme procedures during calculations. A text user interface command is also available,

described in Using the Text User Interface to Define UDFs and Scheme Procedures With Input Para-

meters (p. ).

Overview

Figure . : Use Input Parameter in Scheme Procedure Dialog Box

Use the Select button to open the Select Input Parameter Dialog Box (p. ) where an input para-

meter can be chosen. Enter a Scheme Procedure name or body starting with lambda that should

receive a real argument (the value of the selected input parameter). For example, if the following

Scheme procedure called my-funct is defined as a Scheme file that gets loaded into the current

session,

(define my-funct

(lambda (value )

(ti-menu-load-string (format #f "/solve/set/under-relaxation/pressure ~g" value))))

then enter my-funct for the Scheme Procedure. Otherwise, you can directly enter the following

code for the Scheme Procedure:

(lambda (value)(ti-menu-load-string (args->string '/solve/set/under-relaxation/pressure value)))

Click Define to populate the Registered List. Use Delete to delete the use of the selected input

variable, but not the associated input parameter (the input parameter has to be deleted separately

in the Parameters dialog box). Use Print to print out details of the registered input parameters.

Important

While writing Scheme procedures, you should use the "args->string" help procedure instead

of using double quotes. For example:

(lambda ( value1)

(display (args->string 'Changing-Theta-Divisions-value=   value1))

(ti-menu-load-string

(args->string '/define/models/radiation/discrete-ordinates? 'yes value1  '_  '_  '_)) )

Alternatively, you could also write:

(display (args->string 'Changing-Theta-Divisions-value=  value1))

(apply args->string `(/define/models/radiation/discrete-ordinates? yes ,value1  _  _  _) )) )

where the ` character after args->string is the grave accent character (not a single

quote) and the _ character stores the default value of the current text user interface

prompt. Note that the first occurrence of value1 is the Scheme variable, while the second

occurrence of value1 will be replaced by the value stored in the variable. This method

eliminates the need to specify a single quote for all arguments.

Also note that if you enter a scheme procedure body in the Use Input Parameter in

Scheme Procedure dialog box, you should combine the scheme procedure lines into

one single line.

To use a UDF with input parameters, in the Parameters dialog box under Input Parameters, select

More, then choose Use in UDF to display the Use Input Parameter for UDF Dialog Box (p. ) where

you can register the input parameters that can be used in UDF functions during calculations. A text

user interface command is also available, described in Using the Text User Interface to Define UDFs

and Scheme Procedures With Input Parameters (p. ).

Figure . : Use Input Parameter for UDF Dialog Box

meter can be chosen. Click Define to populate the Registered List. Use Delete to delete the use

of the selected input variable, but not the associated input parameter (the input parameter has to

be deleted separately in the Parameters dialog box). Click Print to print out the parameter ID of

the registered input parameter. This ID should be used to access the value of the parameter in UDF.

By registering the input parameter, ANSYS Fluent knows that this input parameter is being used by

a UDF. In the UDF C function, you can access the registered input parameter value using the

RP_Get_Input_Parameter macro. For example,

Overview

real value = RP_Get_Input_Parameter(“real-”),

where real- is an input parameter ID obtained using the Print feature.

..... Using the Text User Interface to Define UDFs and Scheme Procedures With Input

Parameters

The /define/parameters/input-parameters/advance/use-in text interface command

can also be used to define input parameters and Scheme procedures and user-defined functions.

The Scheme procedures can use other text user interface (TUI) commands in ANSYS Fluent to change

the desired simulation settings in a parametric manner. Each numerical component of the TUI

command string can be marked and treated as a parameter. Setting up advanced input parameters

requires using Scheme functions that use text interface commands to apply new values. Once defined,

these input parameters are displayed in the Parameters dialog box alongside other input parameters.

The input parameter passes a constant numeric value to the registered/provided Scheme function.

Therefore, the associated Scheme function (and corresponding ANSYS Fluent text command) uses

the constant parameter values using the units that were already defined for the designated text

command quantity.

/define/parameters/input-parameters/advance

Enter the advanced input parameters menu.

use-in/

Allows you to use an input parameter in a Scheme procedure or in a UDF.The following examples

demonstrates how to use an input parameter using a Scheme procedure.The Scheme procedure

body can be written at the prompt itself:

/define/parameters/input-parameters/advance> use-in

Select type:> scheme-proc

Name of parameter ["parameter-"]

parameter- value [] .

Enter the name/body of apply-function [()] (lambda (value )

(ti-menu-load-string (format #f "/solve/set/under-relaxation/pressure ~g" value)))

or it can be written in a Scheme file (for example, my-funct)

/define/parameters/custom-input-parameters> use-in

Enter the name/body of apply-function [()] my-funct

where the my-funct Scheme file contents are:

The following example demonstrates how to use an input parameter using a UDF:

Select type:> udf-side

delete

Deletes the use of the selected input variable, but not the associated input parameter (the input

parameter has to be deleted separately). Using the wildcard ‘*’ allows you to delete all custom input

variable at once.

list

Shows usage of input parameters for Scheme procedures and for UDFs

During setup you will want to display boundary conditions, which can be accomplished using the

Mesh Display Dialog Box (p. ). You also have the option to highlight boundaries in the tree, right-

click them, and select Display or Add to Graphics. This feature is particularly useful if you are setting

up a problem for the first time or if you want to visually confirm the location of a particular boundary

condition.

Figure . : Selecting Multiple Boundaries for Display in the Graphics Window

Overview

Conversely, once a mesh or other graphics object is displayed, you can select boundaries using a left

mouse click (use Ctrl or Shift to select multiple boundaries)—the selected boundaries are highlighted

in the tree. The boundary description in the tree includes the zone IDs, which can help you differentiate

the zones. You can also right-click selected boundaries in the graphics window to perform a number

of options including printing information about the boundaries (surface IDs, zone IDs, surface groups,

and so on), fusing zones, and creating graphics objects. For example, refer to Figure . : Example Op-

erations for Multiple Selected Surfaces in the Graphics Window (p. ), which shows some operations

that are available for the selected surfaces (highlighted in light green).

Figure . : Example Operations for Multiple Selected Surfaces in the Graphics Window

The Cell Zone Conditions and Boundary Conditions task pages allow you to access the Operating

Conditions dialog box, where you can set the operating pressure, reference pressure location, include

the effects of gravity, and specify other operating variables, as discussed in Modeling Basic Fluid

Flow (p. ).

Setup →

Cell Zone Conditions → Operating Conditions...

Setup →

Boundary Conditions → Operating Conditions...

The Periodic Conditions dialog box can be accessed from the Boundary Conditions task page. For

a detailed description of this dialog box’s inputs, refer to Periodic Flows (p. ).

Setup →

Boundary Conditions → Periodic Conditions...

To highlight a selected boundary zone of a model that is displayed in the graphics window, enable

the Highlight Zone option in the Boundary Conditions task page.

Important

Important

Note that this is only applicable to 3D cases and is available only in the Boundary Conditions

task page.

There are two ways in which you can highlight a boundary zone in the graphics window, after enabling

the Highlight Zone option:

Select the zone by highlighting it in the Zone list, in the Boundary Conditions task page.

Use the mouse-probe button and select the zone in the graphics window.

The selected zone in the graphics window will be highlighted in a cyan color, which is the default

color. You can change the color using the following text command:

display → set → colors → highlight-color

If you want to highlight a boundary zone that is not displayed in the graphics window, ANSYS Fluent will

display that boundary zone in the graphics window and then highlight it. If you disable the Highlight

Zone option, the displayed boundary zone will be removed from the scene (graphics window) and

your model will be redrawn to its original view.

You can save cell zone and boundary conditions to a file so that you can use them to specify the same

conditions for a different case, as described in Reading and Writing Boundary Conditions (p. ).

Cell zones consist of fluids and solids. Porous zones and 3D fans in ANSYS Fluent are treated as fluid

zones. A detailed description of the various cell zones is given in the sections that follow.

... Fluid Conditions

... Solid Conditions

... Porous Media Conditions

... 3D Fan Zones

... Fixing the Values of Variables

... Locking the Temperature for Solid and Shell Zones

... Defining Mass, Momentum, Energy, and Other Sources

A fluid zone is a group of cells for which all active equations are solved. The only required input for a

fluid zone is the type of fluid material. You must indicate which material the fluid zone contains so

that the appropriate material properties will be used.

Important

If you are modeling multiphase flow, you will not specify the materials here; you will choose

the phase material when you define the phases, as described in Defining the Phases for the

VOF Model (p. ).

Important

If you are modeling species transport and/or combustion, you can specify the material as

either a mixture or a fluid. The mixture material has to be the same as that specified in the

Species Model dialog box when you enable the model. The fluid zones, being of different

material types, must not be contiguous.

Optional inputs allow you to set sources or fixed values of mass, momentum, heat (temperature), tur-

bulence, species, and other scalar quantities. You can also define motion for the fluid zone. If there

are rotationally periodic boundaries adjacent to the fluid zone, you must specify the rotation axis. If

you are modeling turbulence using one of the -  models, the -

model, or the Spalart-Allmaras

model, you can choose to define the fluid zone as a laminar flow region. If you are modeling radiation

using the DO model, you can specify whether or not the fluid participates in radiation.

Warning

In general, disabling Participates in Radiation for fluid zones is not recommended, as it

Warning

can produce erroneous results. There are rare cases when it is acceptable: for example, if

the domain contains multiple fluid zones, disabling this option for zones where radiation

is negligible may save computational time without affecting the results.

Important

For information about porous zones and 3D fan zones, see Porous Media Conditions (p. )

and 3D Fan Zones (p. ), respectively.

.... Inputs for Fluid Zones

You will set all fluid conditions in the Fluid Dialog Box (p. ) (Figure . : The Fluid Dialog Box (p. )),

which is accessed from the Cell Zone Conditions task page (as described in Setting Cell Zone and

Boundary Conditions (p. )).

Figure . : The Fluid Dialog Box

..... Defining the Fluid Material

To define the material contained in the fluid zone, select the appropriate item in the Material Name

drop-down list. This list will contain all fluid materials database) in the Create/Edit Materials Dialog

Box (p. ). If you want to check or modify the properties of the selected material, you can click

Edit... to open the Edit Material dialog box; this dialog box contains just the properties of the se-

lected material, not the full contents of the standard Create/Edit Materials dialog box.

Important

If you are modeling species transport or multiphase flow, the Material Name list will not

appear in the Fluid dialog box. For species calculations, the mixture material for all fluid

zones will be the material you specified in the Species Model Dialog Box (p. ). For

multiphase flows, the materials are specified when you define the phases, as described

in Defining the Phases for the VOF Model (p. ).

..... Defining Sources

If you want to define a source of heat, mass, momentum, turbulence, species, or other scalar

quantity within the fluid zone, you can do so by enabling the Source Terms option. See Defining

Mass, Momentum, Energy, and Other Sources (p. ) for details.

..... Defining Fixed Values

If you want to fix the value of one or more variables in the fluid zone, rather than computing them

during the calculation, you can do so by enabling the Fixed Values option. See Fixing the Values

of Variables (p. ) for details.

..... Specifying a Laminar Zone

When you are calculating a turbulent flow, it is possible to “turn off” turbulence modeling in a spe-

cific fluid zone. To disable turbulence modeling, turn on the Laminar Zone option in the Fluid dialog

box. This is useful if you know that the flow in a certain region is laminar. For example, if you know

the location of the transition point on an airfoil, you can create a laminar/turbulent transition

boundary where the laminar cell zone borders the turbulent cell zone. This feature allows you to

model turbulent transition on the airfoil.

By default, the Laminar Zone option will set the turbulent viscosity,

, to zero and disable turbulence

production in the fluid zone. Turbulent quantities will still be transported through the zone, but effects

on fluid mixing and momentum will be ignored. If you want to keep the turbulent viscosity, you can

do so using the text command define/ boundary-conditions/fluid. You will be asked if

you want to Set Turbulent Viscosity to zero within laminar zone?. If your re-

sponse is no, ANSYS Fluent will set the production term in the turbulence transport equation to

zero, but will retain a nonzero

.

Disabling turbulence modeling in a fluid zone can be applied to all the turbulence models except

the Large Eddy Simulation (LES) model.

..... Specifying a Reaction Mechanism

If you are modeling species transport with reactions, you can enable a reaction mechanism in a fluid

zone by turning on the Reaction option and selecting an available mechanism from the Reaction

Mechanism drop-down list. See Defining Zone-Based Reaction Mechanisms (p. ) for more inform-

ation about defining reaction mechanisms.

..... Specifying the Rotation Axis

If there are rotationally periodic boundaries adjacent to the fluid zone or if the zone is rotating,

either the mesh or its reference frame, you must specify the rotation axis. To define the axis for a

moving reference frame problem, set the Rotation-Axis Direction and Rotation-Axis Origin under

the Reference Frame tab. To define the axis for a moving mesh problem, set the Rotation-Axis

Direction and Rotation-Axis Origin under the Mesh Motion tab.

Note

If a frame motion and a mesh motion are specified at the same zone and this zone

has rotationally periodic boundaries adjacent to it, then both axes have to be coaxial.

Otherwise, the periodicity assumption is not valid and you will receive a warning

message. In addition, the mesh check will fail.

The cell zone axis is independent of the axis of rotation used by any adjacent wall zones or any

other cell zones. For 3D problems, the axis of rotation is the vector from the Rotation-Axis Origin

in the direction of the vector given by your Rotation-Axis Direction inputs for the frame of reference

and the mesh motion. For 2D non-axisymmetric problems, you will specify only the Rotation-Axis

Origin; the axis of rotation is the -direction vector passing through the specified point. (The  dir-

ection is normal to the plane of your geometry so that rotation occurs in the plane.) For 2D

axisymmetric problems, you will not define the axis: the rotation will always be about the  axis,

with the origin at (,).

..... Defining Zone Motion

To define zone motion for a moving reference frame (MRF), enable the Frame Motion option in the

Fluid dialog box. Set the appropriate parameters in the expanded portion of the dialog box, under

the Reference Frame tab.

To define zone motion for a moving (sliding) mesh, enable the Mesh Motion option in the Fluid

dialog box. Set the appropriate parameters in the expanded portion of the dialog box, under the

Mesh Motion tab. See Setting Up the Sliding Mesh Problem (p. ) for details.

For cases that do not contain zones with motion specified in a relative frame to another zone, select

absolute from the Relative To Cell Zone drop-down list. Here, the velocity and rotation components

are specified in an absolute reference frame, which is the default setting, as shown in Figure . : Ro-

tation Specified in the Absolute Reference Frame (p. ). If no moving zones are present in the

simulation, then absolute will be the only available selection. See The Multiple Reference Frame

Model for more information.

Figure . : Rotation Specified in the Absolute Reference Frame

For cases where you have a moving zone specified relative to another moving zone, select the cell

zone carrying the primary motion from the Relative To Cell Zone drop-down list under the Reference

Frame tab or the Mesh Motion tab. Note that for such cases, Rotation-Axis Origin (Relative) will

appear in the interface, signifying coordinates relative to the zone selected from the Relative To

Cell Zone drop-down list.

Figure . : Rotation Specified Relative to a Moving Zone (p. ) illustrates that the rotational axis

origin of the small rotating zone is specified relative to the cell zone carrying the primary motion

(having local coordinate system ).

Figure . : Rotation Specified Relative to a Moving Zone

Note

The Relative To Cell Zone list will consist of all moving cell zones with an absolute motion

specification (that is zones that are moving, but their motion is not relative to some other

zone), excluding the current cell zone.

For problems that include linear, translational motion of the fluid zone, specify the Translational

Velocity by setting the X, Y, and Z components under the Mesh Motion tab. For problems that in-

clude rotational motion, specify the rotational Speed under Rotational Velocity. The rotation axis

is defined as described above. Note that the speed can be specified as a constant value or a transient

profile. The transient profile may be in a file format, as described in Defining Transient Cell Zone

and Boundary Conditions (p. ), or a UDF macro (DEFINE_TRANSIENT_PROFILE). Specifying the in-

dividual velocities as either a profile or a UDF allows you to specify a single component of the frame

motion individually. However, you can also specify the frame motion using a user-defined function.

This may prove to be quite convenient if you are modeling a more complicated motion of the

moving reference frame, where the hooking of many different user-defined functions or profiles can

be cumbersome.

Important

If you need to switch between the MRF and moving mesh models, simply click the Copy

To Mesh Motion for zones with a moving frame of reference and Copy to Frame Motion

for zones with moving meshes to transfer motion variables, such as the axes, frame origin,

and velocity components between the two models. The variables used for the origin, axis,

and velocity components, as well as for the UDF DEFINE_ZONE_MOTION will be copied.

This is particularly useful if you are doing a steady-state MRF simulation to obtain an initial

solution for a transient Moving Mesh simulation in a turbomachine.

See Modeling Flows with Moving Reference Frames (p. ) for details about modeling flows in

moving reference frames. Details about the frame motion UDF can be found in

DEFINE_ZONE_MOTION in the Fluent Customization Manual.

..... Defining Radiation Parameters

If you are using the DO radiation model, you can specify whether or not the fluid zone participates

in radiation using the Participates in Radiation option. See Defining Boundary Conditions for Radi-

ation (p. ) for details.

A “solid” zone is a group of cells for which no flow equations are solved: in a fluid simulation, only a

heat conduction problem is solved; in an intrinsic fluid-structure interaction (FSI) simulation, displace-

ment and stress tensor components are calculated. The material being treated as a solid may actually

be a fluid, but it is assumed that no convection is taking place. The only required input for a solid zone

is the type of solid material. You must indicate which material the solid zone contains so that the ap-

propriate material properties will be used. Optional inputs allow you to set a volumetric heat generation

rate (heat source) or a fixed value of temperature. You can also define motion for the solid zone. If

there are rotationally periodic boundaries adjacent to the solid zone, you must specify the rotation

axis. If you are modeling radiation using the DO model, you can specify whether or not the solid ma-

terial participates in radiation.

.... Inputs for Solid Zones

You will set all solid conditions in the Solid Dialog Box (p. ) (Figure . : The Solid Dialog Box (p. )),

which is opened from the Cell Zone Conditions task page (as described in Setting Cell Zone and

Figure . : The Solid Dialog Box

..... Defining the Solid Material

To define the material contained in the solid zone, select the appropriate item in the Material Name

drop-down list. This list will contain all solid materials database) in the Create/Edit Materials Dialog

..... Defining a Heat Source

If you want to define a source of heat within the solid zone, you can do so by enabling the Source

Terms option. See Defining Mass, Momentum, Energy, and Other Sources (p. ) for details.

..... Defining a Fixed Temperature

If you want to fix the value of temperature in the solid zone, rather than computing it during the

calculation, you can do so by enabling the Fixed Values option. See Fixing the Values of Vari-

ables (p. ) for details.

If there are rotationally periodic boundaries adjacent to the solid zone or if the zone is rotating,

Note

Note

To define rotational motion for a solid, enable the Frame Motion option under Cell Zone Conditions.

Set the appropriate parameters in the expanded portion of the dialog box, under the Reference

Frame tab.

Note that although the user interface implies that solid zone motion is modeled by solving the

equations in a rotating reference frame, it is actually implemented by solving the equations in the

absolute frame using an additional advection term in the solid energy equation. This additional ad-

vection term must be divergence-free, which requires that the specified motion be tangential to the

boundaries. If the motion has a normal component, the solver cannot achieve energy conservation.

The only exception, for which normal motion is permitted, is a coupled wall or mesh interface

between two solid zones having the same material and motion. The solver will print a warning to

the solver transcript the first time it encounters a solid velocity having a significant normal component

at any other boundary type.

The following examples illustrate valid solid zone motion definitions:

Figure . : Single Rotating Solid Zone

Figure . : Rotating solid zone separated from another fluid or solid zone separated by a

surface of revolution.

Figure . : Multiple rotating solid zones having the same material and motion specifications,

separated by mesh interfaces or coupled walls.

The following examples illustrate invalid solid zone motion definitions:

Figure . : Rotating solid with boundaries which are not tangential to the motion.

The following example illustrates a solid motion definition which is formally invalid, but may be ac-

ceptable for engineering purposes:

Figure . : Two solids in contact with some squish. At the contact, the rotational motion has

some normal component, so the solver will not achieve global energy conservation. However,

the temperature field might still be acceptable for engineering purposes.

If the moving solid is separated from a fluid zone by a coupled wall, you must also remember to

specify the wall velocity for the fluid boundary to be consistent with the solid motion.

Limitations:

The effects of solid motion are applied only to the energy equation and the structural model

calculations. User-defined scalars do not include the effects of solid motion.

Only rotating motion can currently be modeled.

Solid motion through a boundary is not permitted; that is, there is no support for a ‘solid inlet’ or

‘solid outlet’.

If you are using the DO radiation model, you can specify whether or not the solid material participates

The porous media model can be used for a wide variety of single phase and multiphase problems,

including flow through packed beds, filter papers, perforated plates, flow distributors, and tube banks.

When you use this model, you define a cell zone in which the porous media model is applied and the

pressure loss in the flow is determined via your inputs as described in Momentum Equations for Porous

Media (p. ). Heat transfer through the medium can also be represented, with or without the assump-

tion of thermal equilibrium between the medium and the fluid flow (as described in Treatment of the

Energy Equation in Porous Media (p. )).

A 1D simplification of the porous media model, termed the “porous jump,” can be used to model a

thin membrane with known velocity/pressure-drop characteristics. The porous jump model is applied

to a face zone, not to a cell zone, and should be used (instead of the full porous media model)

whenever possible because it is more robust and yields better convergence. See Porous Jump

Boundary Conditions (p. ) for details.

.... Limitations and Assumptions of the Porous Media Model

The porous media model incorporates an empirically determined flow resistance in a region of your

model defined as “porous”. In essence, the porous media model adds a momentum sink in the gov-

erning momentum equations. Consequently, the following modeling assumptions and limitations

should be readily recognized:

Since the volume blockage that is physically present is not represented in the model, by default ANSYS

Fluent uses and reports a superficial velocity inside the porous medium, based on the volumetric flow

rate, to ensure continuity of the velocity vectors across the porous medium interface.This superficial ve-

locity formulation does not take porosity into account when calculating the convection and diffusion

terms of the transport equations.You can choose to use a more accurate alternative, in which the true

(physical) velocity is calculated inside the porous medium and porosity is included in the differential terms

of the transport equations. See Modeling Porous Media Based on Physical Velocity (p. ) for details. In

a multiphase flow system, all phases share the same porosity.

The effect of the porous medium on the turbulence field is only approximated. See Treatment of Turbulence

in Porous Media (p. ) for details.

In general, the ANSYS Fluent porous medium model, for both single phase and multiphase, assumes the

porosity is isotropic, and it can vary with space and time.

The Superficial Velocity Formulation and the Physical Velocity Formulation are available for multiphase

porous media. See User Inputs for Porous Media (p. ) for details.

The porous media momentum resistance and heat source terms are calculated separately on each phase.

See Momentum Equations for Porous Media (p. ) for details.

A unique pressure interpolation scheme is always used inside porous media zones regardless of the

pressure scheme selected in the Solution Methods task page.

The interactions between a porous medium and shock waves are not considered.

When applying the porous media model in a moving reference frame, ANSYS Fluent will either apply the

relative reference frame or the absolute reference frame when you enable the Relative Velocity Resistance

Formulation.This allows for the correct prediction of the source terms.

Standard Initialization is the recommended initialization method for porous media simulations.The

default Hybrid Initialization method does not account for the porous media properties, and depending

on boundary conditions, may produce an unrealistic initial velocity field. For porous media simulations,

the Hybrid Initialization method can only be used if the Maintain Constant Velocity Magnitude option

is selected in the Hybrid Initialization dialog box.

The physical velocity porous formulation may produce non-physical flow fields and poor convergence

when porous resistance (Inertial or Viscous) values are less than or comparable to the change in

the dynamic pressure across the porous interface (interior face zone separating the porous and

non-porous cell zone). Switching the porous interface zone to a porous jump boundary is an effective

way to overcome this issue.

.... Momentum Equations for Porous Media

The porous media models for single phase flows and multiphase flows use the Superficial Velocity

Porous Formulation as the default. ANSYS Fluent calculates the superficial phase or mixture velocities

based on the volumetric flow rate in a porous region. The porous media model is described in the

following sections for single phase flow, however, it is important to note the following for multiphase

flow:

In the Eulerian multiphase model (Eulerian Model Theory in the Theory Guide), the general porous media

modeling approach, physical laws, and equations described below are applied to the corresponding phase

for mass continuity, momentum, energy, and all the other scalar equations.

The Superficial Velocity Porous Formulation generally gives good representations of the bulk pressure

loss through a porous region. However, since the superficial velocity values within a porous region remain

the same as those outside the porous region, it cannot predict the velocity increase in porous zones and

therefore limits the accuracy of the model.

Porous media are modeled by the addition of a momentum source term to the standard fluid flow

equations. The source term is composed of two parts: a viscous loss term (Darcy, the first term on

the right-hand side of Equation . (p. ), and an inertial loss term (the second term on the right-

hand side of Equation . (p. ))

(.)

where

is the source term for the  th ( ,

, or ) momentum equation,

is the magnitude of the

velocity and

and  are prescribed matrices. This momentum sink contributes to the pressure

gradient in the porous cell, creating a pressure drop that is proportional to the fluid velocity (or velocity

squared) in the cell.

To recover the case of simple homogeneous porous media

(.)

where  is the permeability and

is the inertial resistance factor, simply specify

and  as diagonal

matrices with

and

, respectively, on the diagonals (and zero for the other elements).

ANSYS Fluent also allows the source term to be modeled as a power law of the velocity magnitude:

(.)

where

and

are user-defined empirical coefficients.

Important

In the power-law model, the pressure drop is isotropic and the units for

are SI.

..... Darcy’s Law in Porous Media

In laminar flows through porous media, the pressure drop is typically proportional to velocity and

the constant

can be considered to be zero. Ignoring convective acceleration and diffusion, the

porous media model then reduces to Darcy’s Law:

(.)

The pressure drop that ANSYS Fluent computes in each of the three ( ,

,

) coordinate directions

within the porous region is then

(.)

where

are the entries in the matrix

in Equation . (p. ),

are the velocity components

in the ,

, and  directions, and

,

, and

are the thicknesses of the medium in the ,

, and  directions.

where

in the ,

,

, and

Here, the thickness of the medium (

,

, or

) is the actual thickness of the porous region

in your model. Therefore if the thicknesses used in your model differ from the actual thicknesses,

you must make the adjustments in your inputs for

.

..... Inertial Losses in Porous Media

At high flow velocities, the constant

in Equation . (p. ) provides a correction for inertial losses

in the porous medium. This constant can be viewed as a loss coefficient per unit length along the

flow direction, thereby allowing the pressure drop to be specified as a function of dynamic head.

If you are modeling a perforated plate or tube bank, you can sometimes eliminate the permeability

term and use the inertial loss term alone, yielding the following simplified form of the porous media

equation:

(.)

or when written in terms of the pressure drop in the ,

,

directions:

(.)

Again, the thickness of the medium (

,

, or

) is the thickness you have defined in your

model.

.... Relative Viscosity in Porous Media

For viscous flows, an effective viscosity,

, is introduced to account for the effect of the porous me-

dium on the diffusion term in the momentum equations:

(.)

where  is the fluid viscosity and

is the relative viscosity. In Fluent the following sub-models are

implemented to calculate the relative viscosity. The effective viscosity is then calculated from Equa-

tion . (p. ).

Brinkman Correction[] (p. )

(.)

Einstein Formula[] (p. )

(.)

Breugem Correlation [] (p. )

(.)

....Treatment of the Energy Equation in Porous Media

(.)

(.)

(.)

ANSYS Fluent solves the standard energy transport equation (Equation . in the Theory Guide) in

porous media regions with modifications to the conduction flux and the transient terms only.

..... Equilibrium Thermal Model Equations

For simulations in which the porous medium and fluid flow are assumed to be in thermal equilibrium,

the conduction flux in the porous medium uses an effective conductivity and the transient term in-

cludes the thermal inertia of the solid region on the medium:

(.)

where

= total fluid energy

= total solid medium energy

= fluid density

= solid medium density

= porosity of the medium

= effective thermal conductivity of the medium

= fluid enthalpy source term

The effective thermal conductivity in the porous medium,

, is computed by ANSYS Fluent as the

volume average of the fluid conductivity and the solid conductivity:

(.)

where

= fluid phase thermal conductivity (including the turbulent contribution,

)

= solid medium thermal conductivity

The fluid thermal conductivity

and the solid thermal conductivity

can be computed via user-

defined functions.

The anisotropic effective thermal conductivity can also be specified via user-defined functions. In

this case, the isotropic contributions from the fluid,

, are added to the diagonal elements of the

solid anisotropic thermal conductivity matrix.

..... Non-Equilibrium Thermal Model Equations

For simulations in which the porous medium and fluid flow are not assumed to be in thermal equi-

librium, a dual cell approach is used. In such an approach, a solid zone that is spatially coincident

with the porous fluid zone is defined, and this solid zone only interacts with the fluid with regard

to heat transfer. The conservation equations for energy are solved separately for the fluid and solid

zones. The conservation equation solved for the fluid zone is

(.)

and the conservation equation solved for the solid zone is

(.)

where

)

= heat transfer coefficient for the fluid / solid interface

= interfacial area density, that is, the ratio of the area of the fluid / solid interface

and the volume of the porous zone

= temperature of the fluid

= temperature of the solid medium

= solid enthalpy source term

The source term due to the non-equilibrium thermal model is represented in Equation . (p. )

and Equation . (p. ) by

and

....Treatment of Turbulence in Porous Media

ANSYS Fluent will, by default, solve the standard conservation equations for turbulence quantities in

the porous medium. In this default approach, turbulence in the medium is treated as though the

solid medium has no effect on the turbulence generation or dissipation rates. This assumption may

be reasonable if the medium’s permeability is quite large and the geometric scale of the medium

does not interact with the scale of the turbulent eddies. In other instances, however, you may want

to suppress the effect of turbulence in the medium.

If you are using one of the turbulence models (with the exception of the Large Eddy Simulation (LES)

model), you can suppress the effect of turbulence in a porous region by enabling the Laminar Zone

option in the Fluid Dialog Box (p. ). Refer to Specifying a Laminar Zone (p. ) for details about

using the Laminar Zone option.

.... Effect of Porosity on Transient Scalar Equations

For transient porous media calculations, the effect of porosity on the time-derivative terms is accounted

for in all scalar transport equations and the continuity equation. When the effect of porosity is taken

into account, the time-derivative term becomes

, where

is the scalar quantity ( , , and

so on) and  is the porosity.

The effect of porosity is enabled automatically for transient calculations, and the porosity is set to

by default.

.... Modeling Porous Media Based on Physical Velocity

As stated in Limitations and Assumptions of the Porous Media Model (p. ), by default ANSYS Flu-

ent calculates the superficial velocity based on volumetric flow rate. The superficial velocity in the

governing equations can be represented as

(.)

(.)

where  is the porosity of the media defined as the ratio of the volume occupied by the fluid to the

total volume.

The superficial velocity values within the porous region remain the same as those outside of the

porous region, and porosity is not taken into account in the differential terms of the transport equa-

tions. This limits the accuracy of the porous model in cases where there should be an increase in ve-

locity throughout the porous region, and does not yield accurate results when velocity values and

gradients are important. For more accurate simulations of porous media flows, it becomes necessary

to solve for the true, or physical, velocity throughout the flowfield rather than the superficial velocity,

as well as to include porosity in all terms of the transport equations.

ANSYS Fluent allows the calculation of the physical velocity using the Porous Formulation, available

in the Cell Zone Conditions task page. By default, the Superficial Velocity option is turned on.

..... Single Phase Porous Media

Using the physical velocity formulation, and assuming a general scalar

, the governing equation

in an isotropic porous media has the following form:

(.)

Assuming isotropic porosity and single phase flow, the volume-averaged mass and momentum

conservation equations are as follows:

(.)

(.)

The last term in Equation . (p. ) represents the viscous and inertial drag forces imposed by the

pore walls on the fluid.

Important

Note that even when you solve for the physical velocity in Equation . (p. ), the two

Important

resistance coefficients can still be derived using the superficial velocity as given in Defining

the Viscous and Inertial Resistance Coefficients (p. ). ANSYS Fluent assumes that the

inputs for these resistance coefficients are based upon well-established empirical correla-

tions that are usually based on superficial velocity. Therefore, ANSYS Fluent automatically

converts the inputs for the resistance coefficients into those that are compatible with the

physical velocity formulation.

Important

Note that the inlet mass flow is also calculated from the superficial velocity. Therefore,

for the same mass flow rate at the inlet and the same resistance coefficients, for either

the physical or superficial velocity formulation you should obtain the same pressure drop

across the porous media zone.

..... Multiphase Porous Media

You can simulate porous media multiphase flows using the Physical Velocity Porous Formulation

to solve the true or physical velocity field throughout the entire flow field, including both porous

and non-porous regions. In this approach, assuming a general scalar in the

phase,

, the gov-

erning equation in an isotropic porous medium takes on the following form:

(.)

Here  is the porosity, which may vary with time and space;

is the phase density;

is the volume

fraction;

is the phase velocity vector;

is the source term; and

is the diffusion coefficient.

The general scalar equation Equation . (p. ) applies to all other transport equations in the Eu-

lerian multiphase model, such as the granular phase momentum and energy equations, turbulence

modeling equations, and the species transport equations.

Assuming isotropic porosity and multiphase flows, the governing equations in the

phase, Equa-

tion ., Equation ., and Equation . in the Theory Guide take the general forms described

below.

......The Continuity Equation

(.)

......The Momentum Equation

(.)

where

is capillary pressure for the wetting phase,

is phase shear stress,

is the body force,

and

are the mass transfers from phase  to phase  and vice versa,

is the absolute per-

meability, and

is the relative permeability. The term in the brackets is the porous sink, having

zero value in non-porous flows/regions. The last two terms includes the general interphase momentum

exchange forces:

is the drag force for non-porous flows/regions,

is the turbulent dispersed

force,

and

are the relative velocity vectors, and

,

, and

are the external body, lift

and virtual mass exchange forces. If the capillary pressure model is not enabled,

=.

Details about the user inputs related to the momentum resistance sources can be found in User Inputs

for Porous Media (p. ).

......The Energy Equation

(.)

where:

Subscripts ,

, and  denote phase , phase , and the solid material, respectively

is the total enthalpy

is the thermal conductivity

is the heat transfer between phase  and phase

is the density

is the heat source

is the phase volume fraction

is the phase velocity

and

are the total enthalpy differences between phases  and  and vice versa

.... User Inputs for Porous Media

and

When you are modeling a porous region, the additional inputs for the problem setup are as follows.

Optional inputs are indicated as such.

. Define the porous zone (as described in Defining the Porous Zone (p. )).

. (optional) Define the porous velocity formulation in the Cell Zone Conditions task page (as described

in Defining the Porous Velocity Formulation (p. )).

. Identify the fluid material flowing through the porous medium (as described in Defining the Fluid Passing

Through the Porous Medium (p. )).

. Enable reactions for the porous zone, if appropriate, and select the reaction mechanism (as described

in Enabling Reactions in a Porous Zone (p. )).

. Enable the Relative Velocity Resistance Formulation. By default, this option is already enabled and

takes the moving porous media into consideration (as described in Including the Relative Velocity Res-

istance Formulation (p. )).

. Set the viscous resistance coefficients (

in Equation . (p. ), or

in Equation . (p. )) and

the inertial resistance coefficients (

in Equation . (p. )), and define

the direction vectors for which they apply. Alternatively, specify the coefficients for the power-law

model. (See Defining the Viscous and Inertial Resistance Coefficients (p. ) for more details.)

. Specify the porosity of the porous medium (as described in Defining Porosity (p. )).

. (optional) Specify the settings for heat transfer (as described in Specifying the Heat Transfer Set-

tings (p. )).

. (optional) Specify a model for relative viscosity (as described in Specifying the Relative Viscosity (p. )).

. (optional, Eulerian multiphase models only) Specify relative permeability (as described in Specifying the

Relative Permeability (p. ).

. (optional) Set the volumetric heat generation rate in the non-solid portion of the porous medium (or

any other sources, such as mass or momentum). (See Defining Sources (p. ) for more details.)

. (optional) Set any fixed values for solution variables in the fluid region (as described in Defining Fixed

Values (p. ).

. Suppress the turbulent viscosity in the porous region, if appropriate. (See Suppressing the Turbulent

Viscosity in the Porous Region (p. ) for more details.)

. Specify the rotation axis and/or zone motion, if relevant. (See Specifying the Rotation Axis and Defining

Zone Motion (p. ) for more details.)

Methods for determining the resistance coefficients and/or permeability are presented below. If you

choose to use the power-law approximation of the porous-media momentum source term, you will

enter the coefficients

and

in Equation . (p. ) instead of the resistance coefficients and flow

You will set all parameters for the porous medium in the Fluid Dialog Box (p. ) (Figure . : The

Fluid Dialog Box for a Porous Zone (p. )), which is opened from the Cell Zone Conditions task

page (as described in Setting Cell Zone and Boundary Conditions (p. )).

Figure . : The Fluid Dialog Box for a Porous Zone

..... Defining the Porous Zone

As mentioned in Overview (p. ), a porous zone is modeled as a special type of fluid zone. To in-

dicate that the fluid zone is a porous region, enable the Porous Zone option in the Fluid dialog

box. The dialog box will expand to show the porous media inputs (as shown in Figure . : The

Fluid Dialog Box for a Porous Zone (p. )).

In a coupled analysis involving Fluent and System Coupling, a porous jump boundary of zero-thickness

next to the porous zone can be used to transfer data between the porous zone and the System

Coupling system. For more about System Coupling and the variable transferred from a porous jump

boundary, see Performing System Coupling Simulations Using Fluent (p. ).

..... Defining the Porous Velocity Formulation

The Cell Zone Conditions task page contains a Porous Formulation region where you can instruct

ANSYS Fluent to use either a superficial or physical velocity in the porous medium simulation. By

default, the velocity is set to Superficial Velocity. For details about using the Physical Velocity

formulation, see Modeling Porous Media Based on Physical Velocity (p. ).

..... Defining the Fluid Passing Through the Porous Medium

To define the fluid that passes through the porous medium, select the appropriate fluid in the Ma-

terial Name drop-down list in the Fluid Dialog Box (p. ). If you want to check or modify the

properties of the selected material, you can click Edit... to open the Edit Material dialog box; this

dialog box contains just the properties of the selected material, not the full contents of the standard

Create/Edit Materials dialog box.

Important

appear in the Fluid dialog box. For species calculations, the mixture material for all flu-

id/porous zones will be the material you specified in the Species Model Dialog Box (p. ).

For multiphase flows, the materials are specified when you define the phases, as described

..... Enabling Reactions in a Porous Zone

If you are modeling species transport with reactions, you can enable reactions in a porous zone by

turning on the Reaction option in the Fluid dialog box and selecting a mechanism in the Reaction

Mechanism drop-down list.

If your mechanism contains wall surface reactions, you also must specify a value for the Surface-to-

Volume Ratio. This value is the surface area of the pore walls per unit volume (

), and can be

thought of as a measure of catalyst loading. With this value, ANSYS Fluent can calculate the total

surface area on which the reaction takes place in each cell by multiplying

by the volume of the

cell and the porosity. See Defining Zone-Based Reaction Mechanisms (p. ) for details about defining

reaction mechanisms. See Wall Surface Reactions and Chemical Vapor Deposition (p. ) for details

about wall surface reactions.

Note

The wall surface reactions in porous medium are allowed only for the pressure-based

solver.

..... Including the Relative Velocity Resistance Formulation

For cases involving moving meshes, dynamic meshes or moving reference frames (MRF), the Relative

solver.

Velocity Resistance Formulation option allows you to better predict porous media sources. The

porous media source terms are calculated using relative velocities in the porous zone. For more in-

formation, see Momentum Equations for Porous Media (p. ). The Relative Velocity Resistance

Formulation option works well for cases with moving and stationary porous media. It is turned on

Note the following limitation when using the Relative Velocity Resistance Formulation option:

The relative velocity resistance formulation is not supported with axisymmetric-swirl when there are

non-zero swirl resistances.

Note

In ANSYS Fluent ., this option was only supported for moving mesh and MRF (with the

exception of power law for modeling porous sources). Currently, this option also supports

dynamic mesh and takes care of proper treatment of porous sources using power law.

..... Defining the Viscous and Inertial Resistance Coefficients

The viscous and inertial resistance coefficients are both defined in the same manner. The basic ap-

proach for defining the coefficients using a Cartesian coordinate system is to define one direction

vector in 2D or two direction vectors in 3D, and then specify the viscous and/or inertial resistance

coefficients in each direction. In 2D, the second direction, which is not explicitly defined, is normal

to the plane defined by the specified direction vector and the  direction vector. In 3D, the third

direction is normal to the plane defined by the two specified direction vectors. For a 3D problem,

the second direction must be normal to the first. If you fail to specify two normal directions, the

solver will ensure that they are normal by ignoring any component of the second direction that is

in the first direction. You should therefore be certain that the first direction is correctly specified.

You can also define the viscous and/or inertial resistance coefficients in each direction using a user-

defined function (UDF). The user-defined options become available in the corresponding drop-down

list when the UDF has been created and loaded into ANSYS Fluent. Note that the coefficients defined

in the UDF must utilize the DEFINE_PROFILE macro. For more information on creating and using

user-defined function, see the Fluent Customization Manual.

If you are modeling axisymmetric swirling flows, you can specify an additional direction component

for the viscous and/or inertial resistance coefficients. This direction component is always tangential

to the other two specified directions. This option is available for both density-based and pressure-

based solvers.

In 3D, it is also possible to define the coefficients using a conical (or cylindrical) coordinate system,

as described below.

Important

Note that the viscous and inertial resistance coefficients are generally based on the super-

ficial velocity of the fluid in the porous media.

The procedure for defining resistance coefficients is as follows:

. Define the direction vectors.

To use a Cartesian coordinate system, simply specify the Direction- Vector and, for 3D, the Direction-

Vector.The unspecified direction will be determined as described above.These direction vectors

correspond to the principle axes of the porous media.

Note

The units for the inertial resistance coefficients (Direction- Vector and Direction-

Vector) is the inverse of length. Should you want to define different units, you

can do so by opening the Units dialog box and selecting resistance from the

Quantities list.

For some problems in which the principal axes of the porous medium are not aligned with

the coordinate axes of the domain, you may not know a priori the direction vectors of the

porous medium. In such cases, the plane tool in 3D (or the line tool in 2D) can help you to

determine these direction vectors.

a.

“Snap” the plane tool (or the line tool) onto the boundary of the porous region. (Follow the in-

structions in Using the Plane Tool (p. ) or Using the Line Tool (p. ) for initializing the tool to

a position on an existing surface.)

b. Rotate the axes of the tool appropriately until they are aligned with the porous medium.

c.

Once the axes are aligned, click the Update From Plane Tool or Update From Line Tool button

in the Fluid dialog box. ANSYS Fluent will automatically set the Direction- Vector to the direction

of the red arrow of the tool, and (in 3D) the Direction- Vector to the direction of the green arrow.

To use a conical coordinate system (for example, for an annular, conical filter element), follow the

steps below.This option is available only in 3D cases.

a.

Turn on the Conical option.

b. Set the Cone Half Angle (the angle between the cone’s axis and its surface, shown in Fig-

ure . : Cone Half Angle (p. )).To use a cylindrical coordinate system, set the Cone Half Angle

to .

c.

Specify the Cone Axis Vector and Point on Cone Axis.The cone axis is specified as being in the

direction of the Cone Axis Vector (unit vector), and passing through the Point on Cone Axis.

The cone axis may or may not pass through the origin of the coordinate system.

Figure . : Cone Half Angle

For some problems in which the axis of the conical filter element is not aligned with the co-

ordinate axes of the domain, you may not know a priori the direction vector of the cone axis

and coordinates of a point on the cone axis. In such cases, the plane tool can help you to de-

termine the cone axis vector and point coordinates. One method is as follows:

a.

Select a boundary zone of the conical filter element that is normal to the cone axis vector in the

drop-down list next to the Snap to Zone button.

b. Click the Snap to Zone button. ANSYS Fluent will automatically “snap” the plane tool onto the

boundary. It will also set the Cone Axis Vector and the Point on Cone Axis. (Note that you will

still have to set the Cone Half Angle yourself.)

An alternate method is as follows:

a.

“Snap” the plane tool onto the boundary of the porous region. (Follow the instructions in Using

the Plane Tool (p. ) for initializing the tool to a position on an existing surface.)

a.

b. Rotate and translate the axes of the tool appropriately until the red arrow of the tool is pointing

in the direction of the cone axis vector and the origin of the tool is on the cone axis.

c.

Once the axes and origin of the tool are aligned, click the Update From Plane Tool button in the

Fluid dialog box. ANSYS Fluent will automatically set the Cone Axis Vector and the Point on

Cone Axis. (Note that you will still have to set the Cone Half Angle yourself.)

. Under Viscous Resistance, specify the viscous resistance coefficient

in each direction.

Under Inertial Resistance, specify the inertial resistance coefficient

in each direction. (You

can scroll down with the scroll bar to view these inputs.)

For porous media cases containing highly anisotropic inertial resistances, enable Alternative

Formulation under Inertial Resistance. The Alternative Formulation option provides better

stability to the calculation when your porous medium is anisotropic. The pressure loss through

the medium depends on the magnitude of the velocity vector of the ith component in the medium.

Using the formulation of Equation . (p. ) yields the expression below:

(.)

Whether or not you use the Alternative Formulation option depends on how well you can fit

your experimentally determined pressure drop data to the ANSYS Fluent model. For example, if

the flow through the medium is aligned with the mesh in your ANSYS Fluent model, then it will

not make a difference whether or not you use the formulation. In general, however, the default

and the Alternative Formulation are not equivalent, and solution differences can occur when

switching between the two options.

For more information about simulations involving highly anisotropic porous media, see Solution

Strategies for Porous Media (p. ).

Important

Note that the alternative formulation is compatible only with the pressure-based

solver.

If you are using the Conical specification method, Direction- is the tangential direction of the

cone, Direction- is the normal to the cone surface (radial ( ) direction for a cylinder), and Dir-

ection- is the circumferential ( ) direction.

In 3D there are three possible categories of coefficients, and in 2D there are two:

In the isotropic case, the resistance coefficients in all directions are the same (for example, a sponge).

For an isotropic case, you must explicitly set the resistance coefficients in each direction to the same

value.

When (in 3D) the coefficients in two directions are the same and those in the third direction are dif-

ferent or (in 2D) the coefficients in the two directions are different, you must be careful to specify the

coefficients properly for each direction. For example, if you had a porous region consisting of cylindrical

straws with small holes in them positioned parallel to the flow direction, the flow would pass easily

through the straws, but the flow in the other two directions (through the small holes) would be very

little. If you had a plane of flat plates perpendicular to the flow direction, the flow would not pass

through them at all; it would instead move in the other two directions.

In 3D the third possible case is one in which all three coefficients are different. For example, if the

porous region consisted of a plane of irregularly-spaced objects (for example, pins), the movement

of flow between the blockages would be different in each direction.You would therefore need to

specify different coefficients in each direction.

Methods for deriving viscous and inertial loss coefficients are described in the sections that follow.

..... Deriving Porous Media Inputs Based on Superficial Velocity, Using a Known

Pressure Loss

When you use the porous media model, you must remember that the porous cells in ANSYS Fluent

are % open, and that the values that you specify for

and/or

must be based on this

assumption. Suppose, however, that you know how the pressure drop varies with the velocity through

the actual device, which is only partially open to flow. The following exercise is designed to show

you how to compute a value for

which is appropriate for the ANSYS Fluent model.

Consider a perforated plate that has % area open to flow. The pressure drop through the plate is

known to be . times the dynamic head in the plate. The loss factor,

, defined as

(.)

is therefore ., based on the actual fluid velocity in the plate, that is, the velocity through the %

open area. To compute an appropriate value for

, note that in the ANSYS Fluent model:

. The velocity through the perforated plate assumes that the plate is % open.

. The loss coefficient must be converted into dynamic head loss per unit length of the porous region.

Noting item , the first step is to compute an adjusted loss factor,

, which would be based on the

velocity of a % open area:

(.)

or, noting that for the same flow rate,

,

(.)

The adjusted loss factor has a value of . Noting item , you must now convert this into a loss

coefficient per unit thickness of the perforated plate. Assume that the plate has a thickness of .

mm (

m). The inertial loss factor would then be

(.)

Note that, for anisotropic media, this information must be computed for each of the  (or ) coordinate

directions.

..... Using the Ergun Equation to Derive Porous Media Inputs for a Packed Bed

As a second example, consider the modeling of a packed bed. In turbulent flows, packed beds are

modeled using both a permeability and an inertial loss coefficient. One technique for deriving the

appropriate constants involves the use of the Ergun equation  [] (p. ), a semi-empirical correlation

applicable over a wide range of Reynolds numbers and for many types of packing:

(.)

When modeling laminar flow through a packed bed, the second term in the above equation may

be dropped, resulting in the Blake-Kozeny equation   [] (p. ):

(.)

In these equations,

is the viscosity,

is the mean particle diameter,

is the bed depth, and  is

the void fraction, defined as the volume of voids divided by the volume of the packed bed region.

Comparing Equation . (p. ) and  Equation . (p. ) with  Equation . (p. ), the permeability

and inertial loss coefficient in each component direction may be identified as

(.)

and

(.)

(.)

and

(.)

..... Using an Empirical Equation to Derive Porous Media Inputs for Turbulent Flow

Through a Perforated Plate

As a third example we will take the equation of Van Winkle et al. [] (p. ) [] (p. ) and show

how porous media inputs can be calculated for pressure loss through a perforated plate with square-

edged holes.

The expression, which is claimed by the authors to apply for turbulent flow through square-edged

holes on an equilateral triangular spacing, is

(.)

where

= mass flow rate through the plate

= the free area or total area of the holes

= the area of the plate (solid and holes)

= a coefficient that has been tabulated for various Reynolds-number ranges and for

various

= the ratio of hole diameter to plate thickness

for

and for

the coefficient  takes a value of approximately ., where the

Reynolds number is based on hole diameter and velocity in the holes.

Rearranging Equation . (p. ), making use of the relationship

(.)

and dividing by the plate thickness,

, we obtain

(.)

where  is the superficial velocity (not the velocity in the holes). Comparing with Equation . (p. )

is seen that, for the direction normal to the plate, the constant

can be calculated from

(.)

..... Using Tabulated Data to Derive Porous Media Inputs for Laminar Flow Through

a Fibrous Mat

Consider the problem of laminar flow through a mat or filter pad which is made up of randomly-

oriented fibers of glass wool. As an alternative to the Blake-Kozeny equation (Equation . (p. ))

we might choose to employ tabulated experimental data. Such data is available for many types of

fiber  [] (p. ).

Dimensionless Permeability  of Glass Wool

Volume Fraction of Solid Material

.

.

.

.

.

.

.

.

.

.

where

and  is the fiber diameter.

, for use in Equation . (p. ), is easily computed for

a given fiber diameter and volume fraction.

..... Deriving the Porous Coefficients Based on Experimental Pressure and Velocity

Data

Experimental data that is available in the form of pressure drop against velocity through the porous

component, can be extrapolated to determine the coefficients for the porous media. To effect a

pressure drop across a porous medium of thickness,

, the coefficients of the porous media are

determined in the manner described below.

If the experimental data is:

Pressure Drop (Pa)

Velocity (m/s)

.

.

.

.

.

.

.

.

then an

curve can be plotted to create a trendline through these points yielding the following

equation

(.)

where

is the pressure drop and  is the velocity.

Important

Although the best fit curve may yield negative coefficients, it should be avoided when

using the porous media model in ANSYS Fluent.

Note that a simplified version of the momentum equation, relating the pressure drop to the source

term, can be expressed as

(.)

or

(.)

Hence, comparing Equation . (p. ) to Equation . (p. ), yields the following curve coefficients:

(.)

with

kg/

, and a porous media thickness,

, assumed to be  m in this example, the

inertial resistance factor,

.

Likewise,

(.)

with

(.)

with

kg/

.

Likewise,

(.)

with

, the viscous inertial resistance factor,

.

Important

Note that this same technique can be applied to the porous jump boundary condition.

Similar to the case of the porous media, you have to take into account the thickness of

the medium

. Your experimental data can be plotted in an

curve, yielding an

equation that is equivalent to Equation . (p. ). From there, you can determine the

permeability  and the pressure jump coefficient

.

..... Using the Power-Law Model

If you choose to use the power-law approximation of the porous-media momentum source term

(Equation . (p. )), the only inputs required are the coefficients

and

. Under Power Law

Model in the Fluid dialog box, enter the values for C0 and C1. Note that the power-law model can

be used in conjunction with the Darcy and inertia models.

C0 must be in SI units, consistent with the value of C1.

..... Defining Porosity

To define the porosity, scroll down below the resistance inputs in the Fluid dialog box, and set the

Porosity under Fluid Porosity. Note that the value of the Porosity must be in the range of –;

furthermore, the lower and upper limits (that is,  and , respectively) are not allowed for the non-

equilibrium thermal model.

You can also define the porosity using a user-defined function (UDF). The user-defined option becomes

available in the corresponding drop-down list when the UDF has been created and loaded into ANSYS

Fluent. Note that the porosity defined in the UDF must utilize the DEFINE_PROFILE macro. For

more information on creating and using user-defined functions, see the separate Fluent Customization

Manual.

The porosity,

, is the volume fraction of fluid within the porous region (that is, the open volume

fraction of the medium). The porosity is used in the prediction of heat transfer in the medium, as

described in Treatment of the Energy Equation in Porous Media (p. ), and in the time-derivative

term in the scalar transport equations for unsteady flow, as described in Effect of Porosity on Transient

Scalar Equations (p. ). It also impacts the calculation of reaction source terms and body forces in

the medium. These sources will be proportional to the fluid volume in the medium. If you want to

represent the medium as completely open (no effect of the solid medium), you should set the

porosity equal to . (the default). When the porosity is equal to ., the solid portion of the medium

will have no impact on heat transfer or thermal/reaction source terms in the medium.

..... Specifying the Heat Transfer Settings

You can model heat transfer in the porous material, with or without the assumption of thermal

equilibrium between the medium and the fluid flow. Note that heat transfer is not available for in-

viscid flow.

...... Equilibrium Thermal Model

To specify that the porous medium and the fluid flow are in thermal equilibrium, scroll down below

the resistance inputs in the Fluid dialog box to the Heat Transfer Settings group box and select

Equilibrium from the Thermal Model list (this is the default selection). Then you must specify the

material contained in the porous medium by selecting the appropriate solid in the Solid Material

Name drop-down list.

If you want to check or modify the properties of the selected material, you can click Edit... to open

the Edit Material dialog box; this dialog box contains just the properties of the selected material,

not the full contents of the standard Create/Edit Materials dialog box. You can define the Thermal

Conductivity of the porous material using a user-defined function (UDF), in order to define a non-

isotropic thermal conductivity. The user-defined option becomes available in the corresponding

drop-down list when the UDF has been created and loaded into ANSYS Fluent. Note that the non-

isotropic thermal conductivity defined in the UDF must utilize the DEFINE_PROPERTY macro. For

more information on creating and using user-defined function, see the separate Fluent Customization

Manual.

...... Non-Equilibrium Thermal Model

Note

The non-equilibrium thermal model is incompatible with the density based solver.

The assumption of thermal equilibrium between the solid medium and the fluid flow is not appro-

priate for all simulations, as the presence of different geometric length scales (for example, pore

sizes) and physical properties of solid and liquid phases may result in local temperature differences

between the phases. Examples of when a non-equilibrium thermal model may be suitable include

the simulation of light-off for exhaust after-treatment, fuel cells, catalytic converters, and so on.

The non-equilibrium thermal model available for porous media in ANSYS Fluent is based on a dual

cell approach. This approach is referred to as “dual cell” because it involves a second solid cell zone

that overlaps (that is, is spatially coincident with) the porous fluid zone; the two zones are solved

simultaneously and are coupled only through heat transfer. ANSYS Fluent can automatically create

a solid zone for you that is a duplicate of the porous fluid zone; otherwise, you can create a duplicate

cell zone manually using the mesh/modify-zones/copy-move-cell-zone text command

before you enable the non-equilibrium thermal model, or make sure that the mesh you read contains

two cell zones in the region where the porous medium will be defined. You should ensure that the

duplicate zone is defined as a solid zone, and that the two zones have similar levels of mesh refine-

ment (as one-to-one mapping will be employed between the cell centroids of the fluid zone and

the solid zone).

Important

When setting up both the porous fluid zone and the overlapping solid zone, note that

the non-equilibrium thermal model is not supported for zones that undergo (or are adja-

cent to zones that undergo) changes to the geometry or mesh, such as dynamic mesh

zones or zones that undergo hanging node adaption, utilize the mesh morpher/optimizer,

or are involved in fluid-structure interaction (FSI) applications.

The instructions that follow assume you have already performed steps – in User Inputs for Porous

Media (p. ). Before you enable the non-equilibrium thermal model, click OK in the Fluid dialog

box, in order to save your settings in the Porous Zone tab; note that if you do not save your settings,

they will be reset to the default values when you enable the non-equilibrium thermal model. Then

reopen the Fluid dialog box and scroll down below the resistance inputs in the Porous Zone tab.

Select Non-Equilibrium from the Thermal Model list in the Heat Transfer Settings group box (see

Figure . : The Heat Transfer Settings Group Box of the Fluid Dialog Box (p. )); this will enable

the dual cell approach and display the associated GUI input controls. If a solid zone that is spatially

coincident with the porous fluid zone does not already exist, use the Question dialog box that opens

to automatically create one. The name of the newly created solid cell zone will then be displayed

in the Solid Zone text box of the Fluid dialog box.

Important

Note that the Non-Equilibrium option button is not available if a radiation and/or mul-

tiphase model is enabled, as such a combination is not supported.

Figure . : The Heat Transfer Settings Group Box of the Fluid Dialog Box

Next, define

and

(as described in Non-Equilibrium Thermal Model Equations (p. )) for Inter-

facial Area Density and Heat Transfer Coefficient, respectively; you can define these settings as

a Constant, a New Input Parameter..., or as a user-defined function. The user-defined option be-

comes available in the corresponding drop-down list when the UDF has been created and loaded

into ANSYS Fluent. Note that the UDF must utilize the DEFINE_PROFILE macro. For more inform-

ation on creating and using user-defined functions, see the separate Fluent Customization Manual.

When you are finished setting up the porous fluid zone, you should verify that the solid zone created

in the previous step has the appropriate settings. Note the name of the zone displayed in the Solid

Zone text box of the Heat Transfer Settings group box (see Figure . : The Heat Transfer Settings

Group Box of the Fluid Dialog Box (p. )), and then double-click that zone in the Zone list of the

Cell Zone Conditions task page to open the Solid dialog box. Then, verify that an appropriate se-

lection is made for Material Name. If you want to check or modify the properties of the selected

material, you can click Edit... to open the Edit Material dialog box; this dialog box contains just the

properties of the selected material, not the full contents of the standard Create/Edit Materials dialog

box. You can define the Thermal Conductivity of the solid material using a user-defined function

(UDF), in order to define a non-isotropic thermal conductivity. The user-defined option becomes

Fluent. Note that the non-isotropic thermal conductivity defined in the UDF must utilize the

DEFINE_PROPERTY macro. For more information on creating and using user-defined functions,

see the separate Fluent Customization Manual.

Note that when postprocessing simulations that utilize the non-equilibrium thermal model, you can

display the energy source due to the temperature difference between the fluid and solid zones using

the Non-Equilibrium Thermal Model Source variable in the Temperature... category. Furthermore,

attention must be paid to the fact that there are overlapping cell zones (that is, a fluid and a solid

zone) in the porous region. For example:

When creating an isosurface and making selections from the From Zones selection list of the Iso-Surface

dialog box, you should never select both the porous fluid zone and the overlapping solid zone at the

same time. Note that if no selections are made in this list, then all the cell zones are selected.

When making selections from the Surfaces list of the Contours dialog box, you should not select a surface

that is associated with the porous fluid zone and a surface associated with the overlapping solid zone

at the same time, if those surfaces are spatially coincident.

When postprocessing the thermal conductivity property in the porous region, the value that is reported

for the fluid zone is the thermal conductivity of the fluid material scaled by the porosity (

) and for the

overlapping solid zone the value reported is the thermal conductivity of the solid zone scaled by the

complement of the porosity (

); where  is the porosity,

is the fluid phase thermal conductivity

(including the turbulent contribution,

), and

is the solid medium thermal conductivity.

..... Specifying the Relative Viscosity

), and

The relative viscosity can be used to account for the effect of the porous media on the diffusion

term in the momentum equation. By default, the relative viscosity is set to a constant value of

(that is, the effective viscosity is equal to the molecular viscosity). You can choose to model the rel-

ative viscosity using one of the models described in Relative Viscosity in Porous Media (p. ), or

you can specify a user-defined function using a DEFINE_PROPERTY macro.

..... Specifying the Relative Permeability

The relative permeability of a phase denotes its ability to transmit the phase material when its sat-

uration (volume fraction) is less than %.

Reservoir engineers often resort to empirical models or measurement curves to determine the relative

and, therefore, the effective permeabilities. In Fluent, the Corey power law model [] (p. ) is

available to account for the relative permeability for the two-phase flow through porous media. The

Corey correlations of the relative permeability can be represented as follows:

(.)

where:

is the reference phase relative permeability

is the normalized saturation in the qth phase

is the Corey exponent for the qth phase

In Fluent the phase saturation is the phase volume fraction. Thus

can be expressed as:

(.)

where

is the volume fraction residual in the qth phase.

For the two-phase oil-water flow example, the relative permeabilities can be obtained from:

(.)

This requires the specification of  parameters:

the reference phase relative permeabilities for the two phases

and

(.)

and

the residual volume fractions for the two phases

and

the Corey exponents for the two phases

and

The Corey correlation is often used for approximation of the relative permeabilities, particularly for

water flooding type scenarios. The relative permeability curves of the oil (or the non-wetting phase)

is usually an S-shaped curve and of the water (or the wetting phase) is a concave upward curve.

Alternatively, if relative permeability data for one or two phases are available as tabular functions

of other solution variables, you can use generic text files to input such data to define phase relative

permeability as described in Specifying Variables in a Tabular Format (p. ).

To model the relative permeability in ANSYS Fluent:

. Set parameters for the mixture phase (mixture is selected for Phase in the Cell Zone Conditions task

page).

a.

In the Fluid dialog box, in the Porous Zone tab, under Relative Permeability, select Corey Model.

Figure . : The Fluid Dialog Box: Relative Permeability

b. From the drop-down lists, select Wetting Phase and Non Wetting Phase.

Important

Although Equation . (p. ) through Equation . (p. ) are valid for any

given phase, care must be exercised in defining the wetting and non-wetting

phases.

. Set conditions for the wetting phase (the wetting phase is selected from the Phase drop-down list in

the Cell Zone Conditions task page). In the Fluid dialog box, in the Porous Zone tab, specify the fol-

lowing parameters in the Wetting Phase Relative Permeability group box:

Minimum Relative Permeability

sets a lower limit for the relative permeability for the wetting phase. A low value increases impact

of the resistance due to relative permeability effects on the flow.This helps to avoid saturation

overshoots and undershoots (that is, phase saturation dropping below residual values) in simulations

carried out for a long period of time.The default value is .e-.The default should work for most

cases, but may be lowered in case undershoot problems persist.

Non-tabular inputs:

Reference Relative Permeability

in Equation . (p. )

Corey Exponent

Residual Saturation

Tabular input:

a.

Select tabular and click Edit....

Note

Prior to using the tabular option, you must read a text file containing phase

relative permeability data as described in Capillary Pressure Data in a Tabular

Format (p. ).

b. In the Table Input dialog box that opens, select the table appropriate for your fluid zone from

the Table List and the names of the columns from the Saturation (VOF) and Relative Permeab-

ility selection lists.

Figure . : The Table Input Dialog Box for Relative Permeability

See Capillary Pressure Data in a Tabular Format (p. ) for details about the text file format.

. Similarly, set conditions for the non-wetting phase (the non-wetting phase is selected from the Phase

drop-down list in the Cell Zone Conditions task page). In the Fluid dialog box, in the Porous Zone

tab, specify the following parameters in the Non Wetting Phase Relative Permeability group:

sets a lower limit for the relative permeability for the non-wetting phase.This item is similar to

Minimum Relative Permeability for the wetting phase.

Non-tabular Inputs:

Tabular Input:

The inputs are similar to the tabular specification for the wetting phase.

On rare occasions, the saturation may still fall below residual saturation. You can fix the affected

phase to its residual saturation and allow the other phase to pass through normally by issuing the

following text commands:

solve/set/multiphase-numerics/porous-media/relative-permeability

enable fix option below residual saturation? [no]

yes

Note

The previous text command is not supported for cases that use the tabular specification

method for phase relative permeability.

..... Specifying the Capillary Pressure

When using the Eulerian multiphase model, you can optionally specify a sub-model for capillary

pressure.

When two or more phases are present in pores, one of the phase (usually water) has a preference

for the pore surfaces. This phase is referred to as the wetting phase, while the other phase is called

the non-wetting phase. The boundary between the phases present in a porous medium is also

curved, due to interfacial tension between the fluid, and this gives rise to a difference in the pressure

across the interface:

(.)

where

and

are the non-wetting and wetting phase pressures, respectively. The difference,

is the capillary pressure. It presents a significant driving force under the conditions of low flow

pressure and high volume fraction.

At the pore scale, capillary pressure depends primarily on the pore geometric characteristics (sizes,

distributions, etc. ), interfacial tensions and wettability (contact angles). At the Macro scale the capillary

pressure is generally assumed to be a function of the saturation of the wetting fluid:

(.)

Its value is often obtained either by measurements or correlations.

In Fluent, the capillary pressure effect is modeled as an additional source term in the wetting phase

using one of the sub-models described below.

...... Brooks-Corey Model

......Van-Genuchten Model

...... Leverett J-Function

...... Skjaeveland Model

...... Capillary Pressure Data in a Tabular Format

...... Capillary Pressure Usage

The Brooks-Corey model [] (p. ) proposed the following relationship for capillary pressure for

primary drainage, in which the porous media initially saturated with water is invaded with oil phase:

(.)

where

is the resulting normalized (effective) saturation:

(.)

where

and

are the minimum and maximum volume fraction (saturation) values, respectively.

By default

and

where

is the residual saturation of phase

The value of

is limited to values greater than . in order to avoid an infinite value for capillary pressure.

In order to solve Equation . (p. ), the entry pressure,

, and the parameter

related to the

pore size are required. The default values in Fluent are

and

which are appro-

priate for air-water flow in sand [] (p. ).

Another well established parametric model was proposed by van Genuchten [] (p. ):

(.)

where

and

(.)

where

is the entry pressure.

is the pore size distribution and

. The default values

inFluent are

and

which are appropriate for air-water flow in sand [] (p. ).

The J-function was developed by Leverett in an attempt to extend the pore-scale capillary pressure

formulation by Washburn [] (p. ) to a Macro-scale capillary pressure model. Leverett proposed

that the averaged pore radius can be expressed in terms of porosity and permeability:

(.)

Furthermore, he acknowledged that the capillary pressure should depend on porosity and permeab-

ility. By analogy to the Washburn equation, he developed a dimensionless J-function [] (p. ):

(.)

(.)

where  is the surface tension,

is the wetting or contact angle, and  and  are fitting parameters.

Various empirical J-functions can be developed to estimate capillary pressure. In the Fluent, the fol-

lowing formulation is used:

(.)

This is the same formulation as is used in the Fluent Fuel Cell Module (see Liquid Water Formation,

Transport, and its Effects (PEMFC Only) in the Fluent Theory Guide).

All of the above-mentioned capillary pressure models (Brooks-Corey, Van-Genuchten, Leverett J-

Function) are limited to primary drainage processes. Water saturation decreases in a primary drainage

process. To model a displacement process where flooding is important, such as water-drive, models

that describe imbibition are required. However, most reservoirs are mixed wettabilty and for these

systems a more comprehensive model that describes both drainage and imbibition processes is re-

quired. The Skjaeveland model for capillary pressure encompasses these features.

The Skjaeveland model [] (p. ) for capillary pressure treats the two fluids symmetrically for

wettability. The Skjaeveland capillary pressure curve is defined by Equation . (p. ).

(.)

Where

is the capillary pressure of the

phase,

and

are fitting parameters,

and

are constants, and

and

are the volume fractions of the two phases.

and

subscripts refer

to wetting and non-wetting phases, respectively.

The positive part of the capillary pressure curve is defined by

and

.

and

define the

negative portion of the capillary pressure curve. The effects of varying

,

,

, and

on the

capillary pressure curve are shown in Figure . : Skjaeveland Correlation Behavior []  (p. ).

Figure . : Skjaeveland Correlation Behavior [] (p. )

Figure . : Skjaeveland Correlation Behavior []  (p. ) shows that there is a lot of flexibility in

the capillary pressure curve. You can add further flexibility to the capillary pressure curve by estim-

ating the residual oil saturation. Note that by varying

and

you can modify the cross-over point

(while keeping

and

unchanged).

Default Value

Parameter

.e5

.e5

.

.

Often, field data for capillary pressure are available as tabular functions of other solution variables.

In, ANSYS Fluent, you can use a tabular method to specify capillary pressure. Multiple files can be

used to specify zone-specific properties, for example, different models for capillary pressure for dif-

ferent zones.

The text file format and the table reading procedure are described in Specifying Variables in a Tab-

ular Format (p. ). Row  and all consecutive rows of the table must contain data points of the

saturation and the corresponding capillary pressure values as a function of the saturation.

See Capillary Pressure Usage (p. ) for more information on tabular input for capillary pressure.

....... Specifying Variables in a Tabular Format

When the tabular input option is available for a solution variable, you can specify the variable as a

tabular function of other solution quantities using one or more generic text files. The tabular method

uses a bisection algorithm along with local linear interpolation to find the value of the tabulated

quantity.

An example of the data file for the capillary pressure variable is shown below.

Default-Skjaevland-Model

Sw          Pc

. .

. .

. .

. .

. .

. .

. .

. .

The text file can be any tab- (or space-) delimited file and must contain the following entries:

Row  – The name of the table. The name should not exceed  characters and contain no spaces.

For example, Default-Skjaevland-Model and Default_Skjaevland_Model are acceptable

names.

Row  – Column names for the table input data (Sw and Pc in the above example).

Row  and all consecutive rows – Data points. Note that although there are no limits on the number

of rows and columns, the files are intended to be relatively small (a few hundred data points max-

imum), since they will be stored as part of the case file.

Each row in the table must be terminated by a newline or carriage return with no space or tab fol-

lowing the last entry in the row.

You must provide an adequate number of data points in order to obtain meaningful results for in-

terpolated variables. The values of the interpolated quantity appearing in the first and last rows of

the table are used as its lower and upper bounds, respectively.

To read the table into ANSYS Fluent:

. In the User-Defined ribbon tab, click Read Table (User-Defined group).

User-Defined → User-Defined → Read Table

. In the Table File Manager dialog box that opens, click Read....

. Use the Select File dialog box to select the file containing the capillary pressure data to be read.

Once ANSYS Fluent loads the file, the table name appears in the Tables selection list in the Table

File Manager dialog box (see Figure . : The Table File Manager Dialog Box (p. )). The table at-

tributes, such as the table type and number of rows and columns, are displayed in the Info field.

Figure . : The Table File Manager Dialog Box

You can add or delete tables at any time by using the Read... or  Delete... buttons.

Unlike locally stored files, these tables, once read in, are written out as part of the Fluent case file.

You do not have to maintain local copies of the tables.

To model the capillary pressure:

.

In the Fluid dialog box for the phase mixture, in the Porous Zone tab, select Corey Model (Model

Options group box).

.

.

.

Select a model from the drop-down list under Capillary Pressure.You can choose from the following

models:

brooks-corey

van-genuchten

leverett-j-function

skjaeveland

tabular

Note that prior to using the tabular option, you must load a text file containing capillary

pressure data as described in Capillary Pressure Data in a Tabular Format (p. ).

.

(tabular only) In the Table Input dialog box that opens when you select tabular, select the table ap-

propriate for your fluid zone from the Table List and the names of the columns from the Saturation

(VOF) and Capillary Pressure selection lists.

Figure . : The Table Input Dialog Box for Capillary Pressure

For details about capillary pressure table files, see Capillary Pressure Data in a Tabular

Note

You can also define capillary pressure as a tabular function by using the text com-

mands available under define/boundary-conditions/set/fluid. Once you

enter mixture for domain id/name, you can select the capillary-pressure

TUI option, set the method to tabular and specify its parameters.

.

Specify Maximum Capillary Pressure.

The capillary pressure graph exhibits asymptotic behavior at the residual saturation of wetting

and non-wetting phases where the capillary pressure approaches plus and minus infinity (see

Figure . : The Activate Cell Zones Dialog Box (p. )). For this reason, the capillary pressure

must be limited to avoid numerical problems.

.

(Brooks-Corey model only) In the secondary phase Fluid dialog box, in the Porous Zone tab, specify

.

the model-specific parameters (Brooks-Corey Model Inputs group box):

Entry pressure

is

in Equation . (p. ).

Pore size exponent

is the parameter

.

(Van-Genuchten model only) In the secondary phase Fluid dialog box, in the Porous Zone tab, specify

the model-specific parameters (Van-Genuchten Model Inputs group box):

is

is

.

(Skjaeveland model only) In the Fluid dialog boxes for the primary and secondary phases, in the Porous

Zone tab, specify the model-specific parameters (Skjaeveland Model Inputs group box):

is a constant

for the wetting phase and

for the non-wetting phase in Equation . (p. ).

is

.

(Leverett J-Function model only) Specify the following model-specific parameters:

. In the Fluid dialog boxes for the secondary phase, in the Porous Zone tab, in the Leverett J-

Function Model Inputs group box, specify Contact Angle (

in Equation . (p. )).

. In the Phase Interaction dialog boxes, in the Surface Tension tab, specify Surface Tension

Coefficient (  in Equation . (p. )).

Alternatively, you can specify a user-defined function that calculates the capillary pressure using a

DEFINE_EXCHANGE_PROPERTY macro.

Note

When modeling the capillary pressure, you should ensure that the wetting phases are

chosen as the secondary phases.

Postprocessing

The following additional field variable is available for secondary phases:

Note that, although this item is available for both non-wetting and wetting phases, meaningful

values are reported only for the wetting phase.

If you want to include effects of the heat generated by the porous medium in the energy equation,

enable the Source Terms option and set a nonzero Energy source. The solver will compute the heat

generated by the porous region by multiplying this value by the total volume of the cells comprising

the porous zone. You may also define sources of mass, momentum, turbulence, species, or other

scalar quantities, as described in Defining Mass, Momentum, Energy, and Other Sources (p. ).

If you want to fix the value of one or more variables in the fluid region of the zone, rather than

computing them during the calculation, you can do so by enabling the Fixed Values option. See

Fixing the Values of Variables (p. ) for details.

..... Suppressing the Turbulent Viscosity in the Porous Region

As discussed in Treatment of Turbulence in Porous Media (p. ), turbulence will be computed in

the porous region just as in the bulk fluid flow. If you are using one of the turbulence models (other

than the Large Eddy Simulation model) and you want the turbulence generation to be zero in the

porous zone, turn on the Laminar Zone option in the Fluid dialog box. Refer to Specifying a Lam-

inar Zone (p. ) for more information about suppressing turbulence generation.

..... Specifying the Rotation Axis and Defining Zone Motion

Inputs for the rotation axis and zone motion are the same as for a standard fluid zone. See Inputs

for Fluid Zones (p. ) for details.

.... Solution Strategies for Porous Media

In general, you can use the standard solution procedures and solution parameter settings when your

ANSYS Fluent model includes porous media. You may find, however, that the rate of convergence

slows when you define a porous region through which the pressure drop is relatively large in the

flow direction (for example, the permeability,

, is low or the inertial factor,

, is large). This slow

convergence can occur because the porous media pressure drop appears as a momentum source

term—yielding a loss of diagonal dominance—in the matrix of equations solved. The best remedy

for poor convergence of a problem involving a porous medium is to supply a good initial guess for

the pressure drop across the medium.

Similarly, Standard Initialization is the recommended initialization method for porous media simu-

lations. The default Hybrid Initialization method does not account for the porous media properties,

and depending on boundary conditions, may produce an unrealistic initial velocity field. For porous

media simulations, the Hybrid Initialization method should only be used with the Maintain Constant

Velocity Magnitude option.

Another possible way to deal with poor convergence is to temporarily disable the porous media

model (by turning off the Porous Zone option in the Fluid Dialog Box (p. )) and obtain an initial

flow field without the effect of the porous region. With the porous media model turned off, ANSYS

Fluent will treat the porous zone as a fluid zone and calculate the flow field accordingly. Once an

initial solution is obtained, or the calculation is proceeding steadily to convergence, you can enable

the porous media model and continue the calculation with the porous region included. (This method

is not recommended for porous media with high resistance.)

Simulations involving highly anisotropic porous media may, at times, pose convergence troubles. You

can address these issues by limiting the anisotropy of the porous media coefficients (

and

)

to two or three orders of magnitude. Even if the medium’s resistance in one direction is infinite, you

do not need to set the resistance in that direction to be greater than  times the resistance in the

primary flow direction.

.... Postprocessing for Porous Media

The impact of a porous region on the flow field can be determined by examining either velocity

components or pressure values. Graphical plots (including XY plots and contour or vector plots) or

alphanumeric reports of the following variables/functions may be of interest:

X, Y, Z Velocity (in the Velocity... category)

Static Pressure (in the Pressure... category)

These variables are contained in the specified categories of the variable selection drop-down list that

appears in postprocessing dialog boxes.

Note that thermal reporting in the porous region is defined as follows:

(.)

where

)

Important

(.)

where

)

Important

For porous media involving surface reactions, you can display/report the surface reaction

rates using the Arrhenius Rate of Reaction-n in the Reactions... category of the variable

selection drop-down list.

Important

Special care must be taken when postprocessing a porous media simulation that utilizes

the non-equilibrium thermal model. See Non-Equilibrium Thermal Model (p. ) for details.

3D fan zones are fluid cell zones that simulate the effect of an axial fan by applying a distributed mo-

mentum source in a toroid-shaped fluid volume (that is, a blade-swept volume). This is in contrast to

fan boundary conditions (for example, a boundary zone of type fan or intake-fan), which are based

on a lumped parameter model in which the fan is considered to be infinitely thin and a discontinuous

pressure rise is specified as a function of velocity. 3D fan zones have the following advantages:

3D fan zones can calculate swirl and radial velocities, as opposed to fan boundary conditions, which are

mainly used to simulate the axial flow and require you to input swirl and radial coefficients.

The results for 3D fan zones can be comparable to moving reference frame (MRF) simulations, and do not

require modeling 3D rotating fan blade geometries.

3D fan zones can simulate a fan even if the available fan curve data was measured at different operating

conditions than that of the simulation.

Note

.... Momentum Equations for 3D Fan Zones

Note

The following equations are used in the 3D fan zone for the momentum sources in the axial, tangential,

and radial directions, which mimic the effect of the fan on the fluid. The tangential momentum source

is based on a turbomachinery relation, whereas the radial momentum source is based on a centrifugal

force balance.

(.)

(.)

(.)

where

= pressure rise across the fan for a given axial flow rate

= thickness of the toroid region swept by the blades in the axial direction

= fan power

= local radial distance from the fan axis

= fan operating angular velocity

= radius of the fan hub

= radius of a point on the fan blade based on the inflection point ratio

= radius of the fan blade tip

= local tangential velocity

In order to calculate the tangential source, three other expressions are necessary:

(.)

(.)

(.)

where

= velocity vector at the fan exit plane

= area vector at the fan exit plane

= the inflection point ratio, that is, the fraction of the fan blade length (starting

at the hub) over which the tangential velocity of the fan discharge is increasing with

increasing radius and peaks, before tapering off (see Figure . : The Inflection Point

Ratio of a Pitched Blade Turbine (p. ))

The pressure rise across the 3D fan zone is specified as a function of the volumetric flow rate through

the fan. The relationship may be a constant or a fan curve, that is, a polynomial or piecewise-linear

function. In the case of a polynomial, the relationship is of the form

(.)

where

(.)

where

are the pressure head polynomial coefficients (calculated by Fluent), and

is the flow rate

normal to the fan.

Important

The flow rate

can be either positive or negative. You must be careful to model the fan

so that a pressure rise occurs for forward flow through the fan.

The fan curve data is typically collected at a prescribed set of test conditions. However, the operating

conditions of your CFD simulation may be inconsistent with this data (for example, the rotational

speed or fluid temperature may be different). To account for this, the 3D fan model can adjust the

fan curve data according to the following scaling relationships:

(.)

(.)

(.)

where

and

are the test temperature and the volume-averaged temperature of the fan cell

zone (which is calculated internally), respectively.

.... User Inputs for 3D Fan Zones

A 3D fan zone is modeled as a special type of fluid zone. The cell zone should have a toroid shape

that is sized to match the blade-swept volume of the fan you are simulating (that is, has an inner and

outer radius that matches the radius of the fan’s hub and blade tips, respectively, as well as a length

that matches the thickness of the toroid region swept by the blades in the axial direction). Furthermore,

the fluid cell zone should be “interior”, that is, have at least two boundary zones of type interior that

border another fluid cell zone and act as the fan inlet and outlet (the other boundaries can be of

type interior as well).

To designate a cell zone as a 3D fan zone, enable the 3D Fan Zone option in the Fluid dialog box

and then define the geometry and properties of the fan in the 3D Fan Zone tab.

Figure . : The Fluid Dialog Box for a 3D Fan Zone

..... Defining the Geometry of a 3D Fan Zone

After enabling the 3D Fan Zone option in the Fluid dialog box, you can begin setting it up by de-

fining the settings in the Geometry group box in the 3D Fan Zone tab of the fluid cell zone:

.

Select a boundary zone from the Inlet Fan Zone drop-down list, which will act as the inlet zone for

the 3D fan zone and the surface on which the fan will be located.This boundary must meet certain

requirements: it must be of type interior; it must be planar; and it must act as a boundary between

the 3D fan zone and another fluid cell zone. Note that the direction the fan blows will be into the 3D

fan zone, perpendicular to this boundary zone.

.

Define the overall dimensions of the fan by entering values for the Hub Radius and the Tip Radius,

as well as the Thickness of the toroid region swept by the blades in the axial direction. Note that the

values must fit within the confines of the 3D fan zone, and that the Thickness will be applied from

the Inlet Fan Zone into the 3D fan zone.

.

Specify the Inflection Point ratio.The inflection point ratio represents the fraction of the fan blade

length (starting at the hub) over which the tangential velocity of the fan discharge is increasing with

increasing radius and peaks, before tapering off. See Figure . :The Inflection Point Ratio of a Pitched

Blade Turbine (p. ) for an illustration.You can derive this ratio empirically from experimental data;

otherwise, you can first use ANSYS Fluent to model the actual fan geometry (for example, using a

moving reference frame simulation) and then use those results to determine the input parameters for

simpler simulations using the 3D Fan Zone option.

Figure . : The Inflection Point Ratio of a Pitched Blade Turbine

.

Enter the coordinates for the Fan Origin.This must define a point that is on the plane of the Inlet Fan

Zone and located such that the diameters of the fan fall within boundaries of the Inlet Fan Zone.

..... Defining the Properties of a 3D Fan Zone

To complete the setup of a 3D fan zone, you must define the settings in the Properties group box

in the 3D Fan Zone tab of the fluid cell zone:

.

Define the Rotational Direction of the fan.The rotation is deemed positive if it follows the right-hand

rule with respect to the fan direction vector (that is, a vector from the Fan Origin that points into the

3D fan zone perpendicular to the Inlet Fan Zone).

.

Specify the Operating Angular Velocity of the fan.This must be a positive nonzero number.

.

You can enable the Limit Flow Rate Through Fan option, and thereby specify the Maximum and

Minimum flow rates that are allowed.

.

You can enable the Tangential Source Term, Radial Source Term, and/or Axial Source Term options,

in order to enable momentum sources in the specified directions. Note that the tangential and radial

sources are defined according to impeller theory, and so no further inputs are necessary, whereas the

axial source term requires additional input (as described in the step that follows).

.

.

If you have enabled the Axial Source Term option, you must define this source in the Axial Source

Term Settings group box. For the Method, you can select one of the following choices:

constant pressure

With this method, you must then specify a constant Pressure Jump that is applied to all of

the cells in the 3D fan zone.

fan curve

This method allows you to specify the pressure jump through a fan curve (pressure rise vs.

volumetric flow rate). Using the Read Fan Curve... button, you can read in a tab-delimited

ASCII file that defines the relationship between pressure and flow rate for the 3D fan cell

zone (see 3D Fan Curve File Format (p. ) for details). You must then specify the Curve Fitting

Method Fluent should use on the data points in your file, selecting either polynomial or

piecewise-linear (for the former, you must then define the Order of Polynomial). Finally,

you must provide an estimate of the Initial Flow Rate through your fan zone, as well as the

Test Angular Velocity and Test Temperature of the experiment that produced the data

points.

Note that a single file can define multiple cell zones, but the file must be read in each of the

applicable Fluid dialog boxes.

.... 3D Fan Zone Limitations

Note the following limitations when setting up a 3D fan zone:

3D fan zones are not supported with the premixed combustion model.

3D fan zones are not supported with the Eulerian multiphase model.

The Energy Equation must be enabled in the Energy Dialog Box (p. ) for 3D fan zones when fan curve

is selected for the axial source term method.

The option to fix values of variables in ANSYS Fluent allows you to set the value of one or more variables

in a fluid or solid zone, essentially setting a boundary condition for the variables within the cells of

the zone. When a variable is fixed in a given cell, the transport equation for that variable is not solved

in the cell (and the cell is not included when the residual sum is computed for that variable). The fixed

value is used for the calculation of face fluxes between the cell and its neighbors. The result is a smooth

transition between the fixed value of a variable and the values at the neighboring cells.

Important

You can fix values for temperature, species mass fractions, and/or velocity components only

if you are using the pressure-based solver. (Refer to Pressure-Based Solver in the Theory

Guide for information about the pressure-based solver.)

.... Overview of Fixing the Value of a Variable

The ability to fix the value of a variable has a wide range of applications. The velocity fixing method

is often used to model the flow in stirred tanks. This approach provides an alternative to the use of

a moving reference frame (solution in the reference frame of the blade) and can be used to model

baffled tanks. In both 2D and 3D geometries, a fluid cell zone may be used in the impeller regions,

and velocity components can be fixed based on measured data.

Although the actual impeller geometry can be modeled and the flow pattern calculated using the

sliding mesh model, experimental data for the velocity profile in the outflow region are available for

many impeller types. If you do not need to know the details of the flow around the blades for your

problem, you can model the impeller by fixing the experimentally-obtained liquid velocities in its

outflow zone. The velocities in the rest of the vessel can then be calculated using this fixed velocity

profile as a boundary condition. Figure . : Fixing Values for the Flow in a Stirred Tank (p. ) shows

an example of how this method is used to model the flow pattern created by a disk-turbine in an

axisymmetric stirred vessel.

Figure . : Fixing Values for the Flow in a Stirred Tank

.....Variables That Can Be Fixed

The variables that can be fixed include velocity components (pressure-based solver only), turbulence

quantities, temperature (pressure-based solver only), enthalpy, species mass fractions (pressure-based

solver only), and user-defined scalars. For turbulence quantities, different values can be set depending

on your choice of turbulence model. You can fix the value of the temperature in a fluid or solid zone

if you are solving the energy equation. If you are using the non-premixed combustion model, you

can fix the enthalpy in a fluid zone. If you have more than one species in your model, you can specify

fixed values for the species mass fractions for each individual species except the last one you defined.

See the Fluent Customization Manual for details about defining user-defined scalars.

If you are using the Eulerian multiphase model, you can fix the values of velocity components and

(depending on which multiphase turbulence model you are using) turbulence quantities on a per-

phase basis. See Eulerian Model (p. ) for details about setting boundary conditions for Eulerian

multiphase calculations.

.... Procedure for Fixing Values of Variables in a Zone

To fix the values of one or more variables in a cell zone, follow these steps (remembering to use only

SI units):

. In the Fluid Dialog Box (p. ) or Solid Dialog Box (p. ), enable the Fixed Values option.

. Fix the values for the appropriate variables in the Fixed Values tab, noting the comments below.

To specify a constant value for a variable, choose constant in the drop-down list next to the relevant

field and then enter the constant value in the field.

To specify a non-constant value for a variable, you can use a profile (see Profiles (p. )) or a user-

defined function for a profile (see the Fluent Customization Manual). Select the appropriate profile or

UDF in the drop-down list next to the relevant field.

If you specify a radial-type profile (see Profile Specification Types (p. )) for temperature, en-

thalpy, species mass/mole fractions, or turbulence quantities for the - , Spalart-Allmaras, or

model, the local coordinate system upon which the radial profile is based is defined by

the Rotation-Axis Origin and Rotation-Axis Direction for the fluid zone. See Specifying the

Rotation Axis (p. ) for information about setting these parameters. (Note that it is acceptable

to specify the rotation axis and direction for a non-rotating zone. This will not cause the zone

to rotate; it will not rotate unless it has been explicitly defined as a moving zone.)

If you do not want to fix the value for a variable, choose (or keep) none in the drop-down list next to

the relevant field.This is the default for all variables.

..... Fixing Velocity Components

To fix the velocity components, you can specify X, Y, and (in 3D) Z Velocity values, or, for axisym-

metric cases, Axial, Radial, and (for axisymmetric swirl) Swirl Velocity values. The units for a fixed

velocity are m/s.

For 3D cases, you can choose to specify cylindrical velocity components instead of Cartesian com-

ponents. Turn on the Local Coordinate System For Fixed Velocities option, and then specify the

Axial, Radial, and/or Tangential Velocity values. The local coordinate system is defined by the

Rotation-Axis Origin and Rotation-Axis Direction for the fluid zone. See Specifying the Rotation

Axis (p. ) for information about setting these parameters. (Note that it is acceptable to specify the

rotation axis and direction for a non-rotating zone. This will not cause the zone to rotate; it will not

rotate unless it has been explicitly defined as a moving zone.)

Important

You can fix values for velocity components only if you are using the pressure-based solver.

(Refer to Pressure-Based Solver in the Theory Guide for information about the pressure-based

solver.)

If all components of velocity are set to fixed values, the solver will also set the gauge pressure

to zero on all cells in the cell zone.

solver.)

..... Fixing Temperature and Enthalpy

If you are solving the energy equation, you can fix the temperature in a zone by specifying the value

of the Temperature. The units for a fixed temperature are K.

If you are using the non-premixed combustion model, you can fix the enthalpy in a zone by specifying

the value of the Enthalpy. The units for a fixed enthalpy are J/kg.

If you specify a radial-type profile (see Profile Specification Types (p. )) for temperature or enthalpy,

the local coordinate system upon which the radial profile is based is defined by the Rotation-Axis

Origin and Rotation-Axis Direction for the fluid zone. See above for details.

Important

You can fix the value of temperature only if you are using the pressure-based solver.

..... Fixing Species Mass Fractions

If you are using the species transport model, you can fix the values of the species mass fractions for

individual species. ANSYS Fluent allows you to fix the species mass fraction for each species (for ex-

ample, h2, o2) except the last one you defined.

If you specify a radial-type profile (see Profile Specification Types (p. )) for a species mass fraction,

Important

You can fix values for species mass fractions only if you are using the pressure-based

solver.

..... Fixing Turbulence Quantities

To fix the values of  and  in the -  equations, specify the Turbulence Kinetic Energy and Tur-

solver.

bulence Dissipation Rate values. The units for  are

/  and those for  are

/ .

To fix the value of the modified turbulent viscosity ( ) for the Spalart-Allmaras model, specify the

Modified Turbulent Viscosity value. The units for the modified turbulent viscosity are

/s.

To fix the values of  and

in the -

equations, specify the Turbulence Kinetic Energy and

Specific Dissipation Rate values. The units for  are

/  and those for

are /s.

To fix the value of , , or the Reynolds stresses in the RSM transport equations, specify the Turbu-

lence Kinetic Energy, Turbulence Dissipation Rate, Specific Dissipation Rate, UU Reynolds Stress,

VV Reynolds Stress, WW Reynolds Stress, UV Reynolds Stress, VW Reynolds Stress, and/or UW

Reynolds Stress. The units for  and the Reynolds stresses are

/ , and those for  are

/ .

If you specify a radial-type profile (see Profile Specification Types (p. )) for , ,

, or , the local

coordinate system upon which the radial profile is based is defined by the Rotation-Axis Origin

and Rotation-Axis Direction for the fluid zone. See above for details. Note that you cannot specify

radial-type profiles for the Reynolds stresses.

..... Fixing User-Defined Scalars

To fix the value of a user-defined scalar, specify the User-defined scalar-n value. (There will be one

for each user-defined scalar you have defined.) The units for a user-defined scalar will be the appro-

priate SI units for the scalar quantity. See the Fluent Customization Manual for information on user-

defined scalars.

You can lock (or “freeze”) the temperature values for all the cells in solid zones (including cells to which

you have applied an energy source using a UDF) and in walls that have shell conduction enabled, so

that the values do not change during further solver iterations. When the temperature is locked for a

given cell, the transport equation will still be solved in the cell, and the cell will be included when the

residual sum is computed.

You can lock / unlock the temperature for solid and shell zones by using the following text command:

solve → set → lock-solid-temperature?

Note the following about the option for locking the temperature of solid and shell zones:

It is only available when energy is enabled and the pressure-based solver is selected.

When this option is used, the BCGSTAB option from the Stabilization Method drop-down list of the Ad-

vanced Solution Controls dialog box is not supported.

Alternative means of monitoring the convergence of energy may be used.

You can define volumetric sources of mass (for single or multiple species), momentum, energy, turbu-

lence, and other scalar quantities in a fluid zone, or a source of energy for a solid zone. This feature is

useful when you want to input a known value for these sources. (For more complicated sources with

functional dependency, you can create a user-defined function as described in the separate Fluent

Customization Manual.) To add source terms to a cell or group of cells, you must place the cell(s) in a

separate zone. The sources are then applied to that cell zone. Typical uses for this feature are listed

below:

A flow source that cannot be represented by an inlet, for example, due to an issue of scale. If you need to

model an inlet that is smaller than a cell, you can place the cell where the tiny “inlet” is located in its own

fluid zone and then define the mass, momentum, and energy sources in that cell zone. For the example

shown in Figure . : Defining a Source for a Tiny Inlet (p. ), you should set a mass source of

and a momentum source of

, where

is the cell volume.

Heat release due to a source (for example, fire) that is not explicitly defined in your model. For this case,

you can place the cell(s) into which the heat is originally released in its own fluid zone and then define the

energy source in that cell zone.

An energy source in a solid zone, for conjugate heat transfer applications. For this case, you can place the

cell(s) into which the heat is originally released in its own solid zone and then define the energy source in

that cell zone.

A species source due to a reaction that is not explicitly included in the model. In the above example of

simulating a fire, you might need to define a source for a species representing smoke generation.

Important

Note that if you define a mass source for a cell zone, you should also define a momentum

source and, if appropriate for your model, energy and turbulence sources. If you define only

a mass source, that mass enters the domain with no momentum or thermal heat. The mass

will therefore have to be accelerated and heated by the flow and, consequently, there may

be a drop in velocity or temperature. This drop may or may not be perceptible, depending

on the size of the source. (Note that defining only a momentum, energy, or turbulence

source is acceptable.)

Figure . : Defining a Source for a Tiny Inlet

.... Sign Conventions and Units

All positive source terms indicate sources, and all negative source terms indicate sinks. All sources

must be specified in SI units.

.... Procedure for Defining Sources

To define one or more source terms for a zone, follow these steps (remembering to use only SI units):

. In the Fluid Dialog Box (p. ) or Solid Dialog Box (p. ), turn on the Source Terms option.

. Set the appropriate source terms under the Source Terms tab, noting the comments below.

To specify a source, click the Edit... button next to the mass, momentum, energy, or other source.The

sources dialog box will open where you will define the number of sources. For each source, choose

none, constant, or New Input Parameter... in the drop-down list.

If you do not want to specify a source term for a variable, choose (or keep) none in the drop-down list

next to the relevant field.This is the default for all variables.

To specify a constant source, choose constant in the drop-down list and then enter the constant value

in the field.

To specify a new source parameter, choose New Input Parameter... in the drop-down list and enter

the Name or the parameter and the Current Value as a constant.

Remember that you should not define just a mass source without defining the other sources, as de-

scribed in Defining Mass, Momentum, Energy, and Other Sources (p. ). above.

Since the sources you specify are defined per unit volume, to determine the appropriate value of your

source term you will often need to first determine the volume of the cell(s) in the zone for which you

are defining the source.To do this, you can use the Volume Integrals Dialog Box (p. ).

..... Mass Sources

If you have only one species in your problem, you can simply define a Mass source for that species.

The units for the mass source are

. In the continuity equation (Equation . in the Theory

Guide), the defined mass source will appear in the

term.

If you have more than one species, you can specify mass sources for each individual species. There

will be a total Mass source term as well as a source term listed explicitly for each species (for example,

h2, o2) except the last one you defined. If the total of all species mass sources (including the last

one) is , then you should specify a value of  for the Mass source, and also specify the values of

the nonzero individual species mass sources. Since you cannot specify the mass source for the last

species explicitly, ANSYS Fluent will compute it by subtracting the sum of all other species mass

sources from the specified total Mass source.

For example, if the mass source for hydrogen in a hydrogen-air mixture is ., the mass source for

oxygen is ., and the mass source for nitrogen (the last species) is ., you will specify a value

of . in the h2 field, a value of . in the o2 field, and a value of . in the Mass field. This

concept also applies within each cell if you use user-defined functions for species mass sources.

The units for the species mass sources are

. In the conservation equation for a chemical

species (Equation . in the Theory Guide), the defined mass source will appear in the

term.

..... Momentum Sources

To define a source of momentum, specify the X Momentum, Y Momentum, and/or Z Momentum

term. The units for the momentum source are N/

. In the momentum equation (Equation . in

the Theory Guide), the defined momentum source will appear in the  term.

..... Energy Sources

To define a source of energy, specify an Energy term. The units for the energy source are W/

. In

the energy equation (Equation . in the Theory Guide), the defined energy source will appear in

the

term.

.....Turbulence Sources

...... Turbulence Sources for the k- ε Model

To define a source of  or  in the -  equations, specify the Turbulent Kinetic Energy or Turbulent

Dissipation Rate term. The units for the  source are kg/m-  and those for  are kg/m- .

The defined  source will appear in the

term on the right-hand side of the turbulent kinetic energy

equation (for example, Equation . in the Theory Guide).

term on the right-hand side of the turbulent dissipation

rate equation (for example, Equation . in the Theory Guide).

......Turbulence Sources for the Spalart-Allmaras Model

To define a source of modified turbulent viscosity, specify the Modified Turbulent Viscosity term.

The units for the modified turbulent viscosity source are kg/m- . In the transport equation for the

Spalart-Allmaras model (Equation . in the Theory Guide), the defined modified turbulent viscosity

source will appear in the

term.

...... Turbulence Sources for the k- ω Model

To define a source of  or

in the -

equations, specify the Turbulent Kinetic Energy or Specific

Dissipation Rate term. The units for the  source are kg/m-  and those for

are kg/

.

equation (Equation . in the Theory Guide).

The defined

term on the right-hand side of the specific turbulent

dissipation rate equation (Equation . in the Theory Guide).

......Turbulence Sources for the Reynolds Stress Model

To define a source of , , or the Reynolds stresses in the RSM transport equations, specify the

Turbulence Kinetic Energy, Turbulence Dissipation Rate, Specific Dissipation Rate, UU Reynolds

Stress, VV Reynolds Stress, WW Reynolds Stress, UV Reynolds Stress, VW Reynolds Stress, and/or

UW Reynolds Stress terms. The units for the  source and the sources of Reynolds stress are kg/m- ,

and those for  are kg/m- .

The defined Reynolds stress sources will appear in the

term on the right-hand side of the

Reynolds stress transport equation (Equation . in the Theory Guide).

term on the right-hand side of Equation . in the

Theory Guide.

The defined  will appear in the

term on the right-hand side of Equation . in the Theory

Guide.

..... Mean Mixture Fraction and Variance Sources

To define a source of the mean mixture fraction or its variance for the non-premixed combustion

model, specify the Mean Mixture Fraction or Mixture Fraction Variance term. The units for the

mean mixture fraction source are

, and those for the mixture fraction variance source are

.

The defined mean mixture fraction source will appear in the

term in the transport equation for

the mixture fraction (Equation . in the Theory Guide).

The defined mixture fraction variance source will appear in the

term in the transport equation

for the mixture fraction variance (Equation . in the Theory Guide).

If you are using the two-mixture-fraction approach, you can also specify sources of the Secondary

Mean Mixture Fraction and Secondary Mixture Fraction Variance.

..... P- Radiation Sources

To define a source for the P- radiation model, specify the P1 term. The units for the radiation source

are W/

, and the defined source will appear in the

term in Equation . in the Theory Guide.

Note that, if the source term you are defining represents a transfer from internal energy to radiative

energy (for example, absorption or emission), you must specify an Energy source of the same

magnitude as the P1 source, but with the opposite sign, in order to ensure overall energy conserva-

tion.

..... Progress Variable Sources

To define a source of the progress variable for the premixed combustion model, specify the Progress

tion.

Variable term. The units for the progress variable source are kg/

s, and the defined source will

appear in the

..... NO, HCN, and NH3 Sources for the NOx Model

To define a source of NO, HCN, or

for the NOx model, specify the no, hcn, or nh3 term. The

units for these sources are kg/

s, and the defined sources will appear in the

,

, and

terms of Equation ., Equation ., and Equation . in the Theory Guide.

..... User-Defined Scalar (UDS) Sources

You can specify source term(s) for each UDS transport equation you have defined in your model.

See Setting Up UDS Equations in ANSYS Fluent (p. ) for details.

Boundary conditions consist of external, internal, and periodic boundaries. Most of the boundary con-

ditions are discussed in the sections that follow.

... Flow Inlet and Exit Boundary Conditions

... Using Flow Boundary Conditions

... Pressure Inlet Boundary Conditions

...Velocity Inlet Boundary Conditions

... Mass-Flow Inlet Boundary Conditions

... Mass-Flow Outlet Boundary Conditions

... Inlet Vent Boundary Conditions

... Intake Fan Boundary Conditions

... Pressure Outlet Boundary Conditions

... Pressure Far-Field Boundary Conditions

... Outflow Boundary Conditions

... Outlet Vent Boundary Conditions

... Exhaust Fan Boundary Conditions

... Degassing Boundary Conditions

...Wall Boundary Conditions

... Symmetry Boundary Conditions

... Periodic Boundary Conditions

... Axis Boundary Conditions

... Fan Boundary Conditions

... Radiator Boundary Conditions

... Porous Jump Boundary Conditions

You can find details about the following types here:

interface zones: Using Sliding Meshes (p. )

interior zones: Interior Dialog Box (p. )

overset zones: Overset Meshes (p. )

RANS/LES interface zones: Setting Up the Embedded Large Eddy Simulation (ELES) Model (p. )

Note

By default, boundaries are grouped by type, but you also have the option of grouping them

by:

Alphabetical (List View)

Name

Cell Zone (Adjacency)

To change the grouping, right-click the Boundary Conditions branch in the Outline View

tree and select Group By / List View or Name or Adjacency.

Group By → List View | Name | Adjacency

ANSYS Fluent has a wide range of boundary conditions that permit flow to enter and exit the solution

domain. To help you select the most appropriate boundary condition for your application, this section

includes descriptions of how each type of condition is used, and what information is needed for each

one. Recommendations for determining inlet values of the turbulence parameters are also provided.

This section provides an overview of flow boundaries in ANSYS Fluent and how to use them.

ANSYS Fluent provides  types of boundary zone types for the specification of flow inlets and exits:

velocity inlet, pressure inlet, mass-flow inlet, mass-flow outlet, pressure outlet, pressure far-field, outflow,

inlet vent, intake fan, outlet vent, exhaust fan, and degassing.

The inlet and exit boundary condition options in ANSYS Fluent are as follows:

Velocity inlet boundary conditions are used to define the velocity and scalar properties of the flow at inlet

Pressure inlet boundary conditions are used to define the total pressure and other scalar quantities at flow

inlets.

Mass-flow inlet boundary conditions are used in compressible flows to prescribe a mass flow rate at an inlet.

It is not necessary to use mass-flow inlets in incompressible flows because when density is constant, velocity

inlet boundary conditions will fix the mass flow. Like pressure and velocity inlets, other inlet scalars are

also prescribed.

Pressure outlet boundary conditions are used to define the static pressure at flow outlets (and also other

scalar variables, in case of backflow).The use of a pressure outlet boundary condition instead of an outflow

condition often results in a better rate of convergence when backflow occurs during iteration.

Pressure far-field boundary conditions are used to model a free-stream compressible flow at infinity, with

free-stream Mach number and static conditions specified.This boundary type is available only for compress-

ible flows.

Outflow boundary conditions are used to model flow exits where the details of the flow velocity and

pressure are not known prior to solution of the flow problem.They are appropriate where the exit flow is

close to a fully developed condition, as the outflow boundary condition assumes a zero streamwise gradient

for all flow variables except pressure.They are not appropriate for compressible flow calculations.

Inlet vent boundary conditions are used to model an inlet vent with a specified loss coefficient, flow direction,

and ambient (inlet) total pressure and temperature.

Intake fan boundary conditions are used to model an external intake fan with a specified pressure jump,

flow direction, and ambient (intake) total pressure and temperature.

Outlet vent boundary conditions are used to model an outlet vent with a specified loss coefficient and

ambient (discharge) static pressure and temperature.

Exhaust fan boundary conditions are used to model an external exhaust fan with a specified pressure jump

and ambient (discharge) static pressure.

Degassing boundary conditions are used to model a free surface through which dispersed gas bubbles are

allowed to escape, but the continuous liquid phase is not. A typical application is a bubble column in which

you want to reduce computational cost by not including the freeboard region in the simulation.The de-

gassing boundary condition is only available for two-phase liquid-gas flows using the Eulerian multiphase

model.

.... Determining Turbulence Parameters

When the flow enters the domain at an inlet, outlet, or far-field boundary, ANSYS Fluent requires

specification of transported turbulence quantities. This section describes which quantities are needed

for specific turbulence models and how they must be specified. It also provides guidelines for the

most appropriate way of determining the inflow boundary values.

..... Specification of Turbulence Quantities Using Profiles

If it is important to accurately represent a boundary layer or fully-developed turbulent flow at the

inlet, you should ideally set the turbulence quantities by creating a profile file (see Profiles (p. ))

from experimental data or empirical formulas. If you have an analytical description of the profile,

rather than data points, you can either use this analytical description to create a profile file, or create

a user-defined function to provide the inlet boundary information. (See the Fluent Customization

Manual for information on user-defined functions.)

Once you have created the profile function, you can use it as described below:

Spalart-Allmaras model: Choose Modified Turbulent Viscosity or Turbulent Viscosity Ratio in the

Turbulence Specification Method drop-down list and select the appropriate profile name in the drop-

down list next to Turbulent Viscosity or Turbulent Viscosity Ratio. ANSYS Fluent computes the

boundary value for the modified turbulent viscosity, , by combining

with the appropriate values of

density and molecular viscosity.

models: Choose K and Epsilon in the Turbulence Specification Method drop-down list and select

the appropriate profile names in the drop-down lists next to Turbulent Kinetic Energy and Turbulent

Dissipation Rate.

models: Choose K and Omega in the Turbulence Specification Method drop-down list and select

the appropriate profile names in the drop-down lists next to Turbulent Kinetic Energy and Specific

based Reynolds stress models: Choose K and Epsilon in the Turbulence Specification Method drop-

down list and select the appropriate profile names in the drop-down lists next to Turbulent Kinetic

Energy and Turbulent Dissipation Rate. Choose Reynolds-Stress Components in the Reynolds-Stress

Specification Method drop-down list and select the appropriate profile name in the drop-down list next

to each of the individual Reynolds-stress components.

based Reynolds stress models: Choose K and Omega in the Turbulence Specification Method drop-

down list and select the appropriate profile names in the drop-down lists next to Specific Dissipation

Rate. Choose Reynolds-Stress Components in the Reynolds-Stress Specification Method drop-down

list and select the appropriate profile name in the drop-down list next to each of the individual Reynolds-

stress components.

..... Uniform Specification of Turbulence Quantities

In some situations, it is appropriate to specify a uniform value of the turbulence quantity at the

boundary where inflow occurs. Examples are fluid entering a duct, far-field boundaries, or even fully-

developed duct flows where accurate profiles of turbulence quantities are unknown.

In most turbulent flows, higher levels of turbulence are generated within shear layers than enter the

domain at flow boundaries, making the result of the calculation relatively insensitive to the inflow

boundary values. Nevertheless, caution must be used to ensure that boundary values are not so

unphysical as to contaminate your solution or impede convergence. This is particularly true of ex-

ternal flows where unphysically large values of effective viscosity in the free stream can “swamp”

the boundary layers.

You can use the turbulence specification methods described above to enter uniform constant values

instead of profiles. Alternatively, you can specify the turbulence quantities in terms of more convenient

quantities such as turbulence intensity, turbulent viscosity ratio, hydraulic diameter, and turbulence

length scale. The default Turbulence Specification Method is set to Turbulent Viscosity Ratio (for

the Spalart-Allmaras model) or Intensity and Viscosity Ratio (for the -  models, the -

models,

or the RSM). These quantities are discussed further in the following sections.

.....Turbulence Intensity

The turbulence intensity, , is defined as the ratio of the root-mean-square of the velocity fluctuations,

, to the mean flow velocity,

.

A turbulence intensity of % or less is generally considered low and turbulence intensities greater

than % are considered high. Ideally, you will have a good estimate of the turbulence intensity at

the inlet boundary from external, measured data. For example, if you are simulating a wind-tunnel

experiment, the turbulence intensity in the free stream is usually available from the tunnel charac-

teristics. In modern low-turbulence wind tunnels, the free-stream turbulence intensity may be as

low as .%.

For internal flows, the turbulence intensity at the inlets is totally dependent on the upstream history

of the flow. If the flow upstream is under-developed and undisturbed, you can use a low turbulence

intensity. If the flow is fully developed, the turbulence intensity may be as high as a few percent.

The turbulence intensity at the core of a fully-developed duct flow can be estimated from the follow-

ing formula derived from an empirical correlation for pipe flows:

(.)

At a Reynolds number of ,, for example, the turbulence intensity will be %, according to this

formula.

The default value for turbulence intensity is % (medium intensity).

.....Turbulence Length Scale and Hydraulic Diameter

The turbulence length scale, , is a physical quantity related to the size of the large eddies that

contain the energy in turbulent flows.

In fully-developed duct flows,  is restricted by the size of the duct, since the turbulent eddies cannot

be larger than the duct. An approximate relationship between  and the physical size of the duct is

(.)

where  is the relevant dimension of the duct and

ensures consistency with the definition

of the turbulent length scales for one- and two-equation turbulence models. The factor of . is

based on the maximum value of the mixing length in fully-developed turbulent pipe flow, where

is the diameter of the pipe. In a channel of non-circular cross-section, you can base  on the hydraulic

diameter.

If the turbulence derives its characteristic length from an obstacle in the flow, such as a perforated

plate, it is more appropriate to base the turbulence length scale on the characteristic length of the

obstacle rather than on the duct size.

It should be noted that the relationship of Equation . (p. ), which relates a physical dimension

( ) to the turbulence length scale ( ), is not necessarily applicable to all situations. For most cases,

however, it is a suitable approximation.

Guidelines for choosing the characteristic length  or the turbulence length scale  for selected flow

types are listed below:

For fully-developed internal flows, choose the Intensity and Hydraulic Diameter specification method

and specify the hydraulic diameter

in the Hydraulic Diameter field.

For flows downstream of turning vanes, perforated plates, and so on, choose the Intensity and Length

Scale method and specify the characteristic length of the flow opening for  in the Turbulent Length

Scale field.

For wall-bounded flows in which the inlets involve a turbulent boundary layer, choose the Intensity and

Length Scale method and use the boundary-layer thickness,

, to compute the turbulence length

scale, , from

. Enter this value for  in the Turbulence Length Scale field.

.....Turbulent Viscosity Ratio

The turbulent viscosity ratio,

, is directly proportional to the turbulent Reynolds number

(

).

is large (on the order of  to ) in high-Reynolds-number boundary layers,

shear layers, and fully-developed duct flows. However, at the free-stream boundaries of most external

flows,

is fairly small. Typically, the turbulence parameters are set so that

. For internal

flows values up to  are sensible for the turbulent viscosity ratio,

. The default value for the

turbulent viscosity ratio is set to .

To specify quantities in terms of the turbulent viscosity ratio, you can choose Turbulent Viscosity

Ratio (for the Spalart-Allmaras model) or Intensity and Viscosity Ratio (for the -  models, the

models, or the RSM). The default value for the turbulence intensity is set to % (medium intensity)

and the turbulent viscosity ratio,

, has a default value of .

..... Relationships for Deriving Turbulence Quantities

To obtain the values of transported turbulence quantities from more convenient quantities such as

,

, or

, you must typically resort to an empirical relation. Several useful relations, most of which

are used within ANSYS Fluent, are presented below.

..... Estimating Modified Turbulent Viscosity from Turbulence Intensity and Length

Scale

To obtain the modified turbulent viscosity,

, for the Spalart-Allmaras model from the turbulence

intensity, , and length scale, , the following equation can be used. Note that this equation assumes

that there is no viscous damping, that is,

(see Modeling the Turbulent Viscosity in the Theory

Guide).

(.)

This formula is also used in ANSYS Fluent if you select the Intensity and Hydraulic Diameter spe-

cification method with the Spalart-Allmaras model. In this case,  is obtained from Equa-

ensures consistency with the definition of the eddy viscosity for -  and -

turbulence models. The value of

is ..

..... Estimating Turbulent Kinetic Energy from Turbulence Intensity

The relationship between the turbulent kinetic energy,

, and turbulence intensity, , is

(.)

where

is the mean flow velocity.

This relationship is used in ANSYS Fluent whenever the Intensity and Hydraulic Diameter, Intensity

(.)

where

and Length Scale, or Intensity and Viscosity Ratio method is used instead of specifying explicit

values for  and .

..... Estimating Turbulent Dissipation Rate from a Length Scale

If you know the turbulence length scale, , you can determine  from the relationship

(.)

The determination of  was discussed previously.

This relationship is used in ANSYS Fluent whenever the Intensity and Hydraulic Diameter or Intensity

and Length Scale method is used instead of specifying explicit values for  and .

..... Estimating Turbulent Dissipation Rate from Turbulent Viscosity Ratio

The value of  can be obtained from the turbulent viscosity ratio

and  using the following rela-

tionship:

(.)

where

is an empirical constant specified in the turbulence model.

This relationship is used in ANSYS Fluent whenever the Intensity and Viscosity Ratio method is

used instead of specifying explicit values for  and .

..... Estimating Turbulent Dissipation Rate for Decaying Turbulence

If you are simulating a wind-tunnel situation in which the model is mounted in the test section

downstream of a mesh and/or wire mesh screens, you can choose a value of  such that

(.)

where

is the approximate decay of  you want to have across the flow domain (say, % of the

inlet value of ),

is the free-stream velocity, and

is the streamwise length of the flow domain.

Equation . (p. ) is a linear approximation to the power-law decay observed in high-Reynolds-

number isotropic turbulence. Its basis is the exact equation for  in decaying turbulence,

.

.

If you use this method to estimate , you should also check the resulting turbulent viscosity ratio

to make sure that it is not too large, using Equation . (p. ).

Although this method is not used internally by ANSYS Fluent, you can use it to derive a constant

free-stream value of  that you can then specify directly by choosing K and Epsilon in the Turbulence

Specification Method drop-down list. In this situation, you will typically determine  from  using

Equation . (p. ).

..... Estimating Specific Dissipation Rate from a Length Scale

If you know the turbulence length scale, , you can determine

from the relationship

(.)

where

is an empirical constant specified in the turbulence model. The determination of  was

discussed previously.

and Length Scale method is used instead of specifying explicit values for  and

.

..... Estimating Specific Dissipation Rate from Turbulent Viscosity Ratio

can be obtained from the turbulent viscosity ratio

tionship:

(.)

used instead of specifying explicit values for  and

.

..... Estimating Reynolds Stress Components from Turbulent Kinetic Energy

When the RSM is used, if you do not specify the values of the Reynolds stresses explicitly at the inlet

using the Reynolds-Stress Components option in the Reynolds-Stress Specification Method drop-

down list, they are approximately determined from the specified values of . The turbulence is as-

sumed to be isotropic such that

(.)

and

(.)

(no summation over the index ).

ANSYS Fluent will use this method if you select K or Turbulence Intensity in the Reynolds-Stress

Specification Method drop-down list.

..... Specifying Inlet Turbulence for LES

The turbulence intensity value specified at a velocity inlet for LES, as described in Large Eddy Simu-

lation Model (p. ), is used to randomly perturb the instantaneous velocity field at the inlet. It does

not specify a modeled turbulence quantity. Instead, the stochastic components of the flow at the

inlet boundary are accounted for by superposing random perturbations on individual velocity com-

ponents as described in Inlet Boundary Conditions for Scale Resolving Simulations in the Theory

Guide.

Pressure inlet boundary conditions are used to define the fluid pressure at flow inlets, along with all

other scalar properties of the flow. They are suitable for both incompressible and compressible flow

calculations. Pressure inlet boundary conditions can be used when the inlet pressure is known but the

flow rate and/or velocity is not known. This situation may arise in many practical situations, including

buoyancy-driven flows. Pressure inlet boundary conditions can also be used to define a “free” boundary

in an external or unconfined flow.

For an overview of flow boundaries, see Flow Inlet and Exit Boundary Conditions (p. ).

.... Inputs at Pressure Inlet Boundaries

..... Summary

You will enter the following information for a pressure inlet boundary:

type of reference frame

total (stagnation) pressure

total (stagnation) temperature

flow direction

static pressure

turbulence parameters (for turbulent calculations)

radiation parameters (for calculations using the P-, DTRM, DO, surface-to-surface, or MC models)

chemical species mass or mole fractions (for species calculations)

mixture fraction and variance (for non-premixed or partially premixed combustion calculations)

progress variable (for premixed or partially premixed combustion calculations)

discrete phase boundary conditions (for discrete phase calculations)

multiphase boundary conditions (for general multiphase calculations)

open channel flow parameters (for open channel flow calculations using the VOF multiphase model)

acoustic wave model settings

All values are entered in the Pressure Inlet Dialog Box (p. ) (Figure . : The Pressure Inlet Dialog

Box (p. )), which is opened from the Boundary Conditions task page (as described in Setting Cell

Zone and Boundary Conditions (p. )). Note that open channel boundary condition inputs are de-

scribed in Modeling Open Channel Flows (p. ), and acoustic wave model settings are described

in Boundary Acoustic Wave Models (p. ).

Figure . : The Pressure Inlet Dialog Box

...... Pressure Inputs and Hydrostatic Head

When gravitational acceleration is activated in the Operating Conditions dialog box (accessed from

the Boundary Conditions task page), the pressure field (including all pressure inputs) will include

the hydrostatic head. This is accomplished by redefining the pressure in terms of a modified pressure

that includes the hydrostatic head (denoted

) as follows:

(.)

where

is a constant operating density,

is the gravity vector (also a constant), and

(.)

is the position vector. Noting that

(.)

it follows that

(.)

The substitution of this relation in the momentum equation gives pressure gradient and gravitational

body force terms of the form

(.)

where  is the fluid density. Therefore, if the fluid density is constant, we can set the operating

density

equal to the fluid density, thereby eliminating the body force term. If the fluid density is

not constant (for example, density is given by the ideal gas law), then the operating density should

be chosen to be representative of the average or mean density in the fluid domain, so that the body

force term is small.

An important consequence of this treatment of the gravitational body force is that your inputs of

pressure (now defined as

) should not include hydrostatic pressure differences. Moreover, reports

of static and total pressure will not show any influence of the hydrostatic pressure. See Natural

Convection and Buoyancy-Driven Flows (p. ) for additional information.

...... Defining Total Pressure and Temperature

Enter the value for total pressure in the Gauge Total Pressure field in the Pressure Inlet dialog

box. Total temperature is set in the Thermal tab, in the Total Temperature field.

Remember that the total pressure value is the gauge pressure with respect to the operating pressure

defined in the Operating Conditions Dialog Box (p. ). Total pressure for an incompressible fluid

is defined as

(.)

and for a compressible fluid of constant

as

(.)

= total pressure

where

= static pressure

M = Mach number

= ratio of specific heats

If you are modeling axisymmetric swirl,

in Equation . (p. ) will include the swirl component.

The Total Temperature, Gauge Total Pressure, and flow directions are in absolute or relative to

the adjacent cell zone reference frames, based on the Reference Frame setting in the Pressure Inlet

If the cell zone adjacent to a pressure inlet is defined as a moving reference frame zone, and you

are using the pressure-based solver, the velocity in Equation . (p. ) (or the Mach number in

Equation . (p. )) will be absolute or relative to the mesh velocity, depending on whether or

not the Absolute velocity formulation is enabled in the General task page. For the density-based

solver, the Absolute velocity formulation is always used; hence, the velocity in Equation . (p. )

(or the Mach number in Equation . (p. )) is always the Absolute velocity.

For the Eulerian multiphase model, the total temperature, and velocity components must be specified

for the individual phases. The Reference Frame (Relative to Adjacent Cell Zone or Absolute) for

each of the phases is the same as the reference frame selected for the mixture phase. Note that the

total pressure values must be specified in the mixture phase.

Important

Important

If the flow is incompressible, then the temperature assigned in the Pressure Inlet dialog box

will be considered the static temperature.

For the mixture multiphase model, if a boundary allows a combination of compressible and

incompressible phases to enter the domain, then the temperature assigned in the Pressure

Inlet dialog box will be considered the static temperature at that boundary. If a boundary

allows only a compressible phase to enter the domain, then the temperature assigned in the

Pressure Inlet dialog box will be taken as the total temperature (relative/absolute) at that

boundary.The total temperature will depend on the Reference Frame option selected in the

Pressure Inlet dialog box.

For the VOF multiphase model, if a boundary allows a compressible phase to enter the domain,

then the temperature assigned in the Pressure Inlet dialog box will be considered the total

temperature at that boundary.The total temperature (relative/absolute) will depend on the

Reference Frame option chosen in the dialog box. Otherwise, the temperature assigned to

the boundary will be considered the static temperature at the boundary.

For the Eulerian multiphase model, if a boundary allows a mixture of compressible and incom-

pressible phases in the domain, then the temperature of each of the phases will be the total

or static temperature, depending on whether the phase is compressible or incompressible.

Total temperature (relative/absolute) will depend on the Reference Frame option chosen in

the Pressure Inlet dialog box.

...... Defining the Flow Direction

The flow direction is defined as a unit vector ( ) which is aligned with the local velocity vector,

.

This can be expressed simply as

(.)

Important

For the inputs in ANSYS Fluent, the flow direction  need not be a unit vector, as it will

be automatically normalized before it is applied.

Important

For a moving reference frame, the relative flow direction

is defined in terms of the

relative velocity,

. Thus,

(.)

You can define the flow direction at a pressure inlet explicitly, or you can define the flow to be

normal to the boundary. If you choose to specify the direction vector, you can set either the (Cartesian)

,

, and  components, or the (cylindrical) radial, tangential, and axial components.

For moving zone problems calculated using the pressure-based solver, the flow direction will be

absolute or relative to the mesh velocity, depending on whether or not the Absolute velocity for-

mulation is selected in the General task page. For the density-based solver, the flow direction will

always be in the absolute frame.

The procedure for defining the flow direction is as follows (refer to Figure . : The Pressure Inlet

Dialog Box (p. )):

. Specify the flow direction by selecting Direction Vector or Normal to Boundary in the Direction

. If you selected Normal to Boundary in step  and you are modeling axisymmetric swirl, enter the ap-

propriate value for the Tangential-Component of Flow Direction. If you chose Normal to Boundary

and your geometry is 3D or 2D without axisymmetric swirl, there are no additional inputs for flow dir-

ection.

. If you selected Direction Vector in step , and your geometry is 3D, choose Cartesian (X,Y, Z), Cyl-

indrical(Radial,Tangential, Axial), Local Cylindrical (Radial,Tangential, Axial), or Local Cylindrical

Swirl from the Coordinate System drop-down list. Some notes on these selections are provided below:

The Cartesian coordinate option is based on the Cartesian coordinate system used by the geometry.

Enter appropriate values for the X, Y, and Z-Component of Flow Direction.

The Cylindrical coordinate system uses the axial, radial, and tangential components based on the

following coordinate systems:

– For problems involving a single cell zone, the coordinate system is defined by the rotation axis and

origin specified in the Fluid Dialog Box (p. ).

– For problems involving multiple zones (for example, multiple reference frames or sliding meshes),

the coordinate system is defined by the rotation axis specified in the Fluid (or Solid) dialog box

for the fluid (or solid) zone that is adjacent to the inlet.

For all of the above definitions of the cylindrical coordinate system, positive radial velocities

point radially outward from the rotation axis, positive axial velocities are in the direction of

the rotation axis vector, and positive tangential velocities are based on the right-hand rule

using the positive rotation axis (see Figure . : Cylindrical Velocity Components in 3D, 2D,

and Axisymmetric Domains (p. )).

Figure . : Cylindrical Velocity Components in 3D, 2D, and Axisymmetric Domains

The Local Cylindrical coordinate system allows you to define a coordinate system specifically for

the inlet.When you use the local cylindrical option, you will define the coordinate system right here

in the Pressure Inlet dialog box.The local cylindrical coordinate system is useful if you have several

inlets with different rotation axes. Enter appropriate values for the Axial, Radial, and Tangential-

Component of Flow Direction, and then specify the X, Y, and Z components of the Axis Origin and

Axis Direction.

The Local Cylindrical Swirl coordinate system option allows you to define a coordinate system

specifically for the inlet where the total pressure, swirl velocity, and the components of the velocity

in the axial and radial planes are specified. Enter appropriate values for the Axial and Radial-Com-

ponent of Flow Direction, and the Tangential-Velocity. Specify the X, Y, and Z components of the

Axis Origin and Axis Direction. It is recommended that you start your simulation with a smaller swirl

velocity and then progressively increase the velocity to obtain a stable solution.

Important

Local Cylindrical Swirl should not be used for open channel boundary conditions

and on the mixing plane boundaries while using the mixing plane model.

. If you selected Direction Vector in step , and your geometry is 2D, define the vector components as

follows:

For a 2D planar geometry, enter appropriate values for the X, Y, and Z-Component of Flow Direction.

For a 2D axisymmetric geometry, enter appropriate values for the Axial, Radial-Component of Flow

Direction.

For a 2D axisymmetric swirl geometry, enter appropriate values for the Axial, Radial, and Tangential-

Component of Flow Direction.

Figure . : Cylindrical Velocity Components in 3D, 2D, and Axisymmetric Domains (p. ) shows

the vector components for these different coordinate systems.

...... Defining Static Pressure

The static pressure (termed the Supersonic/Initial Gauge Pressure) must be specified if the inlet

flow is supersonic or if you plan to initialize the solution based on the pressure inlet boundary con-

ditions. Solution initialization is discussed in Initializing the Solution (p. ).

Remember that the static pressure value you enter is relative to the operating pressure set in the

Operating Conditions Dialog Box (p. ). Note the comments in Pressure Inputs and Hydrostatic

Head (p. ) regarding hydrostatic pressure.

The Supersonic/Initial Gauge Pressure is ignored by ANSYS Fluent whenever the flow is subsonic,

in which case it is calculated from the specified stagnation quantities. If you choose to initialize the

solution based on the pressure-inlet conditions, the Supersonic/Initial Gauge Pressure will be used

in conjunction with the specified stagnation pressure to compute initial values according to the is-

entropic relations (for compressible flow) or Bernoulli’s equation (for incompressible flow). Therefore,

for a sub-sonic inlet it should generally be set based on a reasonable estimate of the inlet Mach

number (for compressible flow) or inlet velocity (for incompressible flow).

...... Prevent Reverse Flow

When this option is selected, Fluent will erect artificial walls on the boundary mesh faces to prevent

flow out of the domain. The artificial walls are removed when the flow is no longer leaving the domain

and when a favorable pressure gradient is recovered at the boundary mesh faces.

When artificial walls are created, Fluent will print a message in the console window indicating the

number of faces on which artificial walls have been erected and the equivalent area percentage of

the boundary it represents.

Note

This feature is not available with multiphase flow.

...... Defining Turbulence Parameters

For turbulent calculations, there are several ways in which you can define the turbulence parameters.

Instructions for deciding which method to use and determining appropriate values for these inputs

are provided in Determining Turbulence Parameters (p. ). Turbulence modeling in general is de-

scribed in Modeling Turbulence (p. ).

...... Defining Radiation Parameters

If you are using the P-, DTRM, DO, surface-to-surface, or MC models, you will set the Internal

Emissivity and (optionally) External Black Body Temperature. See Defining Boundary Conditions

for Radiation (p. ) for details. (The Rosseland radiation model does not require any boundary

condition inputs.)

...... Defining Species Mass or Mole Fractions

If you are modeling species transport, you will set the species mass or mole fractions under Species

Mole Fractions or Species Mass Fractions. For details, see Defining Cell Zone and Boundary Condi-

tions for Species (p. ).

...... Defining Non-Premixed Combustion Parameters

If you are using the non-premixed or partially premixed combustion model, you will set the Mean

Mixture Fraction and Mixture Fraction Variance (and the Secondary Mean Mixture Fraction and

Secondary Mixture Fraction Variance, if you are using two mixture fractions), as described in De-

fining Non-Premixed Boundary Conditions (p. ).

...... Defining Premixed Combustion Boundary Conditions

If you are using the premixed or partially premixed combustion model, you will set the Progress

Variable, as described in Setting Boundary Conditions for the Progress Variable (p. ).

...... Defining Discrete Phase Boundary Conditions

If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the

pressure inlet. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

...... Defining Multiphase Boundary Conditions

If you are using the VOF, mixture, or Eulerian model for multiphase flow, you will need to specify

volume fractions for secondary phases and (for some models) additional parameters. See Defining

Multiphase Cell Zone and Boundary Conditions (p. ) for details.

...... Defining Open Channel Boundary Conditions

If you are using the VOF model for multiphase flow and modeling open channel flows, you will need

to specify the Free Surface Level, Bottom Level, and additional parameters. See Modeling Open

Channel Flows (p. ) for details.

.... Default Settings at Pressure Inlet Boundaries

Default settings (in SI) for pressure inlet boundary conditions are as follows:

Gauge Total Pressure

Supersonic/Initial Gauge Pressure

Normal to

Boundary

Direction Specification Method

%

Normal to

Boundary

%

.... Calculation Procedure at Pressure Inlet Boundaries

The treatment of pressure inlet boundary conditions by ANSYS Fluent can be described as a loss-free

transition from stagnation conditions to the inlet conditions. For incompressible flows, this is accom-

plished by application of the Bernoulli equation at the inlet boundary. In compressible flows, the

equivalent isentropic flow relations for an ideal gas are used.

..... Incompressible Flow Calculations at Pressure Inlet Boundaries

When flow enters through a pressure inlet boundary, ANSYS Fluent uses the boundary condition

pressure you input as the total pressure of the fluid at the inlet plane,

. In incompressible flow,

the inlet total pressure and the static pressure,

, are related to the inlet velocity via Bernoulli’s

equation:

(.)

With the resulting velocity magnitude and the flow direction vector you assigned at the inlet, the

velocity components can be computed. The inlet mass flow rate and fluxes of momentum, energy,

and species can then be computed as outlined in Calculation Procedure at Velocity Inlet Boundar-

ies (p. ).

For incompressible flows, density at the inlet plane is either constant or calculated as a function of

temperature and/or species mass/mole fractions, where the mass or mole fractions are the values

you entered as an inlet condition.

If flow exits through a pressure inlet, the total pressure specified is used as the static pressure. For

incompressible flows, total temperature is equal to static temperature.

..... Compressible Flow Calculations at Pressure Inlet Boundaries

In compressible flows, isentropic relations for an ideal gas are applied to relate total pressure, static

pressure, and velocity at a pressure inlet boundary. Your input of total pressure,

, at the inlet and

the static pressure,

, in the adjacent fluid cell are therefore related as

(.)

where

(.)

= the speed of sound, and

. Note that the operating pressure,

, appears in Equa-

tion . (p. ) because your boundary condition inputs are in terms of pressure relative to the

operating pressure. Given

and

, Equation . (p. ) and  Equation . (p. ) are used to

compute the velocity magnitude of the fluid at the inlet plane. Individual velocity components at

the inlet are then derived using the direction vector components.

For compressible flow, the density at the inlet plane is defined by the ideal gas law in the form

(.)

For multi-species gas mixtures, the specific gas constant,

, is computed from the species mass or

mole fractions,

that you defined as boundary conditions at the pressure inlet boundary. The

static temperature at the inlet,

, is computed from your input of total temperature,

, as

(.)

Velocity inlet boundary conditions are used to define the flow velocity, along with all relevant scalar

properties of the flow, at flow inlets. In this case, the total (or stagnation) pressure is not fixed but will

rise (in response to the computed static pressure) to whatever value is necessary to provide the pre-

scribed velocity distribution. This boundary condition is applicable to incompressible and compressible

flows.

Important

Use caution when specifying the velocity inlet boundary condition for a compressible fluid

in internal flow modeling. If the flow path is completely choked with no secondary flow

path for relief, the velocity inlet boundary condition is not recommended, as it can cause

numerical instabilities. In this case, you should switch to the pressure inlet boundary condition

or refrain from reaching operating conditions that choke the internal flow. The choking

condition can happen in high speed supersonic and transonic flow.

In special instances, a velocity inlet may be used in ANSYS Fluent to define the flow velocity at flow

exits. (The scalar inputs are not used in such cases.) In such cases you must ensure that overall continuity

is maintained in the domain.

.... Inputs at Velocity Inlet Boundaries

You will enter the following information for a velocity inlet boundary:

velocity magnitude and direction or velocity components

swirl velocity (for 2D axisymmetric problems with swirl)

temperature (for energy calculations)

outflow gauge pressure (for calculations with the density-based solver)

acoustic wave model settings (see Boundary Acoustic Wave Models (p. ))

All values are entered in the Velocity Inlet Dialog Box (p. ) (Figure . : The Velocity Inlet Dialog

Zone and Boundary Conditions (p. )). Note that acoustic wave model settings are described in

Boundary Acoustic Wave Models (p. ).

Figure . : The Velocity Inlet Dialog Box

..... Defining the Velocity

You can define the inflow velocity by specifying the velocity magnitude and direction, the velocity

components, or the velocity magnitude normal to the boundary. If the cell zone adjacent to the

velocity inlet is moving (that is, if you are using a moving reference frame, multiple reference frames,

or sliding meshes), you can specify either relative or absolute velocities. For axisymmetric problems

with swirl in ANSYS Fluent, you will also specify the swirl velocity.

The procedure for defining the inflow velocity is as follows:

. Specify the flow direction by selecting Magnitude and Direction, Components, or Magnitude, Normal

to Boundary in the Velocity Specification Method drop-down list.

. If the cell zone adjacent to the velocity inlet is moving, you can choose to specify relative or absolute

velocities by selecting Relative to Adjacent Cell Zone or Absolute in the Reference Frame drop-down

list. If the adjacent cell zone is not moving, Absolute and Relative to Adjacent Cell Zone will be

equivalent, so you need not visit the list.

. If you are going to set the velocity magnitude and direction or the velocity components, and your

geometry is 3D, choose Cartesian (X,Y, Z), Cylindrical (Radial,Tangential, Axial), or Local Cylindrical

(Radial,Tangential, Axial) from the Coordinate System drop-down list. See Defining the Flow Direc-

tion (p. ) for information about Cartesian, cylindrical, and local cylindrical coordinate systems.

. Set the appropriate velocity parameters, as described below for each specification method.

..... Setting the Velocity Magnitude and Direction

If you selected Magnitude and Direction as the Velocity Specification Method in step  above,

you will enter the magnitude of the velocity vector at the inflow boundary (the Velocity Magnitude)

and the direction of the vector:

If your geometry is 2D non-axisymmetric, or you chose in step  to use the Cartesian coordinate system,

you will define the X, Y, and (in 3D) Z-Component of Flow Direction.

If your geometry is 2D axisymmetric, or you chose in step  to use a Cylindrical coordinate system, enter

the appropriate values of Radial, Axial, and (if you are modeling axisymmetric swirl or using cylindrical

coordinates) Tangential-Component of Flow Direction.

If you chose in step  to use a Local Cylindrical coordinate system, enter appropriate values for the

Axial, Radial, and Tangential-Component of Flow Direction, and then specify the X, Y, and Z compon-

ents of the Axis Origin and the Axis Direction.

..... Setting the Velocity Magnitude Normal to the Boundary

If you selected Magnitude, Normal to Boundary as the Velocity Specification Method in step

above, you will enter the magnitude of the velocity vector at the inflow boundary (the Velocity

Magnitude).

..... Setting the Velocity Components

If you selected Components as the Velocity Specification Method in step  above, you will enter

the components of the velocity vector at the inflow boundary as follows:

you will define the X, Y, and (in 3D) Z-Velocity.

If your geometry is 2D axisymmetric without swirl, you will set the Radial and Axial-Velocity.

If your model is 2D axisymmetric with swirl, you will set the Axial, Radial, and Swirl-Velocity, and (op-

tionally) the Angular Velocity, as described below.

If you chose in step  to use a Cylindrical coordinate system, you will set the Radial, Tangential, and

Axial-Velocity, and (optionally) the Angular Velocity, as described below.

If you chose in step  to use a Local Cylindrical coordinate system, you will set the Radial, Tangential,

and Axial-Velocity, and (optionally) the Angular Velocity, as described below, and then specify the X,

Y, and Z component of the Axis Origin and the Axis Direction.

Important

Remember that positive values for ,

, and  velocities indicate flow in the positive ,

Important

, and  directions. If flow enters the domain in the negative  direction, for example,

you will need to specify a negative value for the  velocity. The same holds true for the

radial, tangential, and axial velocities. Positive radial velocities point radially out from the

axis, positive axial velocities are in the direction of the axis vector, and positive tangential

velocities are based on the right-hand rule using the positive axis.

..... Setting the Angular Velocity

If you chose Components as the Velocity Specification Method in step  above, and you are

modeling axisymmetric swirl, you can specify the inlet Angular Velocity

in addition to the Swirl-

Velocity. Similarly, if you chose Components as the Velocity Specification Method and you chose

in step  to use a Cylindrical or Local Cylindrical coordinate system, you can specify the inlet An-

gular Velocity

in addition to the Tangential-Velocity.

If you specify

,

is computed for each face as

, where  is the radial coordinate in the coordinate

system defined by the rotation axis and origin. If you specify both the Swirl-Velocity and the Angular

Velocity, or the Tangential-Velocity and the Angular Velocity, ANSYS Fluent will add

and

to get the swirl or tangential velocity at each face.

..... Defining Static Pressure

flow is supersonic or if you plan to initialize the solution based on the velocity inlet boundary con-

The Supersonic/Initial Gauge Pressure is ignored by ANSYS Fluent whenever the flow is subsonic.

If you choose to initialize the flow based on the velocity inlet conditions, the Supersonic/Initial

Gauge Pressure will be used in conjunction with the specified stagnation quantities to compute

initial values according to isentropic relations.

Head (p. )

..... Defining the Temperature

For calculations in which the energy equation is being solved, you will set the static temperature of

the flow at the velocity inlet boundary in the Thermal tab in the Temperature field.

..... Defining Outflow Gauge Pressure

If you are using the density-based solver, you can specify an Outflow Gauge Pressure for a velocity

inlet boundary. If the flow exits the domain at any face on the boundary, that face will be treated

as a pressure outlet with the pressure prescribed in the Outflow Gauge Pressure field.

..... Defining Turbulence Parameters

..... Defining Species Mass or Mole Fractions

..... Defining Non-Premixed Combustion Parameters

..... Defining Premixed Combustion Boundary Conditions

..... Defining Discrete Phase Boundary Conditions

velocity inlet. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

..... Defining Multiphase Boundary Conditions

.... Default Settings at Velocity Inlet Boundaries

Default settings (in SI) for velocity inlet boundary conditions are as follows:

X-Component of Flow Direction

Y-Component of Flow Direction

Z-Component of Flow Direction

X-Velocity

Y-Velocity

Z-Velocity

%

Outflow Gauge Pressure

.... Calculation Procedure at Velocity Inlet Boundaries

ANSYS Fluent uses your boundary condition inputs at velocity inlets to compute the mass flow into

the domain through the inlet and to compute the fluxes of momentum, energy, and species through

the inlet. This section describes these calculations for the case of flow entering the domain through

the velocity inlet boundary and for the less common case of flow exiting the domain through the

velocity inlet boundary.

.....Treatment of Velocity Inlet Conditions at Flow Inlets

When your velocity inlet boundary condition defines flow entering the physical domain of the

model, ANSYS Fluent uses both the velocity components and the scalar quantities that you defined

as boundary conditions to compute the inlet mass flow rate, momentum fluxes, and fluxes of energy

and chemical species.

The mass flow rate entering a fluid cell adjacent to a velocity inlet boundary is computed as

(.)

Note that only the velocity component normal to the control volume face contributes to the inlet

mass flow rate.

(.)

.....Treatment of Velocity Inlet Conditions at Flow Exits

Sometimes a velocity inlet boundary is used where flow exits the physical domain. This approach

might be used, for example, when the flow rate through one exit of the domain is known or is to

be imposed on the model.

Important

In such cases you must ensure that overall continuity is maintained in the domain.

In the pressure-based solver, when flow exits the domain through a velocity inlet boundary ANSYS

Fluent uses the boundary condition value for the velocity component normal to the exit flow area.

It does not use any other boundary conditions that you have input. Instead, all flow conditions except

the normal velocity component are assumed to be those of the upstream cell.

In the density-based solver, if the flow exits the domain at any face on the boundary, that face will

be treated as a pressure outlet with the pressure prescribed in the Outflow Gauge Pressure field.

..... Density Calculation

Density at the inlet plane is either constant or calculated as a function of temperature, pressure,

and/or species mass/mole fractions, where the mass or mole fractions are the values you entered

as an inlet condition.

Mass flow boundary conditions can be used in ANSYS Fluent to provide a prescribed mass flow rate

or mass flux distribution at an inlet. As with a velocity inlet, specifying the mass flux permits the total

pressure to vary in response to the interior solution. This is in contrast to the pressure inlet boundary

condition (see Pressure Inlet Boundary Conditions (p. )), where the total pressure is fixed while the

mass flux varies. The mass-flow inlet is applicable to incompressible and compressible flows.

Important

Use caution when specifying the mass-flow inlet boundary condition for a compressible

fluid in internal flow modeling. If the flow path is completely choked with no secondary

flow path for relief, the mass-flow inlet boundary condition is not recommended, as it can

cause numerical instabilities. In this case, you should switch to the pressure inlet boundary

condition or refrain from reaching operating conditions that choke the internal flow. The

choking condition can happen in high speed supersonic and transonic flow.

A mass-flow inlet is often used when it is more important to match a prescribed mass flow rate than

to match the total pressure of the inflow stream. An example is the case of a small cooling jet that is

bled into the main flow at a fixed mass flow rate, while the velocity of the main flow is governed

primarily by a (different) pressure inlet/outlet boundary condition pair. A mass-flow inlet boundary

condition can also be used as an outflow by specifying the flow direction away from the solution domain.

.... Limitations and Special Considerations

The adjustment of inlet total pressure might result in a slower convergence, so if both the pressure inlet

boundary condition and the mass-flow inlet boundary condition are acceptable choices, you should

choose the former.

inlet boundary conditions will fix the mass flow.

.... Inputs at Mass-Flow Inlet Boundaries

You will enter the following information for a mass-flow inlet boundary:

mass flow rate, mass flux, or (primarily for the mixing plane model) mass flux with average mass flux

All values are entered in the Mass-Flow Inlet Dialog Box (p. ) (Figure . : The Mass-Flow Inlet

Dialog Box (p. )), which is opened from the Boundary Conditions task page (as described in

Setting Cell Zone and Boundary Conditions (p. )). Note that open channel boundary condition

inputs are described in Modeling Open Channel Flows (p. ), and acoustic wave model settings

are described in Boundary Acoustic Wave Models (p. ).

Figure . : The Mass-Flow Inlet Dialog Box

..... Selecting the Reference Frame

You will have the option to specify the mass flow boundary conditions either in the absolute or rel-

ative reference frame, when the cell zone adjacent to the mass-flow inlet is moving. For such a case,

choose Absolute (the default) or Relative to Adjacent Cell Zone in the Reference Frame drop-

down list. If the cell zone adjacent to the mass-flow inlet is not moving, both formulations are

equivalent.

..... Defining the Mass Flow Rate or Mass Flux

You can specify the mass flow rate through the inlet zone and have ANSYS Fluent convert this value

to mass flux, or specify the mass flux directly. For cases where the mass flux varies across the

boundary, you can also specify an average mass flux; see below for more information about this

specification method.

You can define the mass flux or mass flow rate using a profile or a user-defined function.

The inputs for mass flow rate or flux are as follows:

. Make a selection in the Mass Flow Specification Method drop-down list to specify whether you will

define a Mass Flow Rate, Mass Flux, or Mass Flux with Average Mass Flux.

. If you selected Mass Flow Rate (the default), enter the prescribed Mass Flow Rate when constant is

selected from the drop-down list. Otherwise, select your hooked user-defined function (UDF) or transient

profile.

Important

The hooked UDF or transient profile can only be used to provide time-varying specific-

ation of mass flow rate. Therefore, the transient solver must be used to run the simu-

lation. Note that the variation of profile with position in space is not applicable with

this hookup.

See DEFINE_PROFILE in the Fluent Customization Manual for an example of a mass-flow inlet

UDF.

Important

Note that for axisymmetric problems, this mass flow rate is the flow rate through the

entire (

radian) domain, not through a -radian slice.

. If you selected Mass Flux, enter the prescribed Mass Flux, or select your hooked UDF or profile.

. If you selected Mass Flux with Average Mass Flux, enter the prescribed Mass Flux and Average Mass

Flux.

Important

Note that for axisymmetric problems, the Mass Flux and Average Mass Flux is the flux

through a -radian slice of the domain.

..... More About Mass Flux and Average Mass Flux

As noted previously, you can specify an average mass flux with the mass flux. If, for example, you

specify a mass flux profile such that the average mass flux integrated over the zone area is ., but

you actually want to have a total mass flux of , you can keep the profile unchanged, and specify

an average mass flux of . ANSYS Fluent will maintain the profile shape but adjust the values so that

the resulting mass flux across the boundary is .

The mass flux with average mass flux specification method is also used by the mixing plane model

described in The Mixing Plane Model (p. ). If the mass-flow inlet boundary is going to represent

one of the mixing planes, then you do not need to specify the mass flux or flow rate; you can keep

the default Mass Flow Rate of . When you create the mixing plane later on in the problem setup,

ANSYS Fluent will automatically select the Mass Flux with Average Mass Flux method in the Mass-

Flow Inlet dialog box and set the Average Mass Flux to the value obtained by integrating the mass

flux profile for the upstream zone. This will ensure that mass is conserved between the upstream

zone and the downstream (mass-flow inlet) zone.

..... Defining the Total Temperature

Enter the value for the total (stagnation) temperature of the inflow stream in the Total Temperature

field in the Thermal tab.

The total temperature is specified either in the absolute reference frame or relative to the adjacent

cell zone, depending on your setting for the Reference Frame.

For the Eulerian multiphase model, the total temperature, and mass flux components need to be

specified for the individual phases. The Reference Frame (Relative to Adjacent Cell Zone or Abso-

lute) for each of the phases is the same as the reference frame selected for the mixture phase.

Important

Note that you can only set the reference frame for the mixture, however, the total tem-

perature can only be set for the individual phases.

Important

If the flow is incompressible, then the temperature assigned in the Mass-Flow Inlet dialog

box is considered to be the static temperature.

incompressible phases to enter the domain, then the temperature assigned in the Mass-Flow

Inlet dialog box is considered to be the static temperature at that boundary. If a boundary

Mass-Flow Inlet dialog box is the total temperature (relative/absolute) at that boundary.The

total temperature depends on the Reference Frame option selected in the Mass-Flow Inlet

then the temperature assigned in the Mass-Flow Inlet dialog box is considered to be the

total temperature at that boundary.The total temperature (relative/absolute) depends on the

the boundary is considered to be the static temperature at the boundary.

pressible phases in the domain, then the temperature of each of the phases is the total or

static temperature, depending on whether the phase is compressible or incompressible.Total

temperature (relative/absolute) depends on the Reference Frame option chosen in the Mass-

Flow Inlet dialog box.

If you choose to initialize the flow based on the mass-flow inlet conditions, the Supersonic/Initial

..... Defining the Flow Direction

You can define the flow direction at a mass-flow inlet explicitly, or you can define the flow to be

normal to the boundary.

The procedure for defining the flow direction is as follows, referring to Figure . : The Mass-Flow

Inlet Dialog Box (p. ):

. If you selected Direction Vector and your geometry is 2D, go to the next step. If your geometry is 3D,

choose Cartesian (X,Y, Z), Cylindrical (Radial,Tangential, Axial), Local Cylindrical (Radial,Tangen-

tial, Axial), or Local Cylindrical Swirl in the Coordinate System drop-down list. See Defining the Flow

Direction (p. ) for information about Cartesian, cylindrical, local cylindrical, and local cylindrical swirl

coordinate systems.

. If you selected Direction Vector, set the vector components as follows:

If your geometry is 2D non-axisymmetric, or you chose to use a 3D Cartesian coordinate system,

enter appropriate values for the X-, Y-, and (in 3D) Z-Component of Flow Direction.

If your geometry is 2D axisymmetric, or you chose to use a 3D Cylindrical coordinate system, enter

appropriate values for the Axial-, Radial-, and (if you are modeling swirl or using cylindrical coordin-

ates) Tangential-Component of Flow Direction.

If you chose to use a 3D Local Cylindrical coordinate system, enter appropriate values for the Axial-,

Radial-, and Tangential-Component of Flow Direction, and then specify the X, Y, and Z components

of Axis Origin and the Axis Direction.

If you chose to use a 3D Local Cylindrical Swirl coordinate system, enter appropriate values for the

Axial- and Radial-Component of Flow Direction in the axial and radial planes, and the Tangential-

Velocity. Specify the X, Y, and Z components of the Axis Origin and the Axis Direction.

Important

and on the mixing plane boundaries, while using the mixing plane model.

. If you selected Normal to Boundary, there are no additional inputs for flow direction.

Important

Note that if you are modeling axisymmetric swirl, the flow direction will be normal to

the boundary; that is, there will be no swirl component at the boundary for axisym-

metric swirl.

are provided in Determining Turbulence Parameters (p. ). Turbulence modeling is described in

Modeling Turbulence (p. ).

mass-flow inlet. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

..... Defining Open Channel Boundary Conditions

.... Default Settings at Mass-Flow Inlet Boundaries

Default settings (in SI) for mass-flow inlet boundary conditions are as follows:

Mass Flow Rate

%

.... Calculation Procedure at Mass-Flow Inlet Boundaries

When mass flow boundary conditions are used for an inlet zone, a velocity is computed for each face

in that zone, and this velocity is used to compute the fluxes of all relevant solution variables into the

domain. With each iteration, the computed velocity is adjusted so that the correct mass flow value

is maintained.

To compute this velocity, your inputs for mass flow rate, flow direction, static pressure, and total

temperature are used.

There are two ways to specify the mass flow rate. The first is to specify the total mass flow rate,

,

for the inlet. The second is to specify the mass flux,

(mass flow rate per unit area). If a total mass

flow rate is specified, ANSYS Fluent converts it internally to a uniform mass flux by dividing the mass

flow rate by the total inlet area:

(.)

If the direct mass flux specification option is used, the mass flux can be varied over the boundary by

using profile files or user-defined functions. If the average mass flux is also specified (either explicitly

by you or automatically by ANSYS Fluent), it is used to correct the specified mass flux profile, as de-

scribed earlier in this section.

Once the value of

at a given face has been determined, the density,

, at the face must be de-

termined in order to find the normal velocity,

. The manner in which the density is obtained depends

upon whether the fluid is modeled as an ideal gas or not. Each of these cases is examined below.

..... Flow Calculations at Mass Flow Boundaries for Ideal Gases

If the fluid is an ideal gas, the static temperature and static pressure are required to compute the

density:

(.)

If the inlet is supersonic, the static pressure used is the value that has been set as a boundary con-

dition. If the inlet is subsonic, the static pressure is extrapolated from the cells inside the inlet face.

The static temperature at the inlet is computed from the total enthalpy, which is determined from

the total temperature that has been set as a boundary condition. The total enthalpy is given by

(.)

where the velocity magnitude is related to the mass flow rate given by Equation . (p. ) and

the known user-specified flow direction vector. Using Equation . (p. ) to relate density to the

(known) static pressure and (unknown) temperature, Equation . (p. ) can be solved to obtain

the static temperature.

..... Flow Calculations at Mass Flow Boundaries for Incompressible Flows

When you are modeling incompressible flows, the static temperature is equal to the total temperature.

The density at the inlet is either constant or readily computed as a function of the temperature and

(optionally) the species mass or mole fractions. The velocity is then computed using Equa-

..... Flux Calculations at Mass Flow Boundaries

To compute the fluxes of all variables at the inlet, the flux velocity,

, is used along with the inlet

value of the variable in question. For example, the flux of mass is

, and the flux of turbulence

kinetic energy is

. These fluxes are used as boundary conditions for the corresponding conser-

vation equations during the course of the solution.

Mass-flow outlet boundaries can be used in ANSYS Fluent to pump flow out of the domain at a pre-

scribed mass flow rate or mass flux distribution. A mass-flow outlet is often used when it is more im-

portant to match a prescribed mass flow rate than to match the static pressure of the outflow stream.

Mass-flow outlet boundaries have the following limitations:

It is supported with single-phase flow only, and so is not supported with the VOF, mixture, and Eulerian

multiphase models in the pressure-based solver.

It is not supported with the Wet Steam model in the density-based solver.

.... Inputs at Mass-Flow Outlet Boundaries

You will enter the following information for a mass-flow outlet boundary:

mass flow rate, mass flux, mass flux with average mass flux, or exit corrected mass flow rate with reference

temperature and gauge pressure

All values are entered in the Mass-Flow Outlet Dialog Box (p. ) (Figure . : The Mass-Flow Outlet

Setting Cell Zone and Boundary Conditions (p. )).

Figure . : The Mass-Flow Outlet Dialog Box

Mass-flow outlets only support the Relative to Adjacent Cell Zone specification for the Reference

Frame.

You can specify the mass flow rate through the outlet zone and have ANSYS Fluent convert this

value to mass flux, or specify the mass flux directly. For cases where the mass flux varies across the

boundary, you can specify an average mass flux. For compressible problems, you can specify that

the mass flow rate is adjusted to total conditions at the outlet, thus maintaining a constant exit

corrected mass flow rate.

You can define the mass flow or mass flux rate using a profile or a user-defined function (UDF). For

an example of a mass-flow outlet UDF, see DEFINE_PROFILE in the Fluent Customization Manual.

Important

The hooked UDF or transient profile can only be used to provide time-varying specification

of mass flow or mass flux rate. Therefore, the transient solver must be used to run the

simulation. Note that the variation of profile with position in space is not applicable with

define a Mass Flow Rate, Mass Flux, Mass Flux with Average Mass Flux, or (if the density of the ma-

terial is defined either as an ideal gas or using a real gas model) Exit Corrected Mass Flow Rate.

profile.

. If you selected Mass Flux, enter the prescribed Mass Flux (or select your hooked UDF or profile).

. If you selected Mass Flux with Average Mass Flux, enter the prescribed Mass Flux (or select your

hooked UDF or profile) and Average Mass Flux.

Note that if you specify a mass flux profile such that the average mass flux integrated over the

zone area is ., but you actually want to have a total mass flux of , you can keep the profile

unchanged, and specify an average mass flux of . ANSYS Fluent will maintain the profile shape

but adjust the values so that the resulting mass flux across the boundary is .

. If you selected Exit Corrected Mass Flow Rate, enter the prescribed Exit Corrected Mass Flow Rate

(or select your hooked UDF or profile); this corresponds to

in Equation . (p. ).Then enter the

ECMF Reference Temperature (

) and the ECMF Reference Gauge Pressure (

). For complete

details about this method, see Exit Corrected Mass Flow Rate (p. ).

Important

Note that for axisymmetric problems:

If you provide a mass flow rate, you must specify the flow rate through the entire (

radian)

domain, not through a -radian slice.

Important

radian)

If you provide a mass flux rate, you must specify the flux through a -radian slice of the domain.

The mass flow boundary will be pumping flow out of the domain normal to the boundary at the

prescribed rate or flux. If the mass flow rate is specified, then by default, the fluxes on the boundary

will be allowed to vary to preserve the flow profile out of the domain. At convergence, the total

mass flow rate should match the specified value.

Important

Note that if constant mass flux is needed rather than the default variable fluxes to preserve

the profiles, then you can do so via the text command define/boundary-condi-

tions/bc-settings/mass-flow. Answer no when asked to preserve profile

while flow leaves.

Note

The mass-flow outlet boundary condition is designed to be strictly used only when flow

is leaving the domain; it should not be used for mixed flow conditions (where flow is

flowing in and out) or when flow is changing directions.

mass-flow outlet. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

.... Default Settings at Mass-Flow Outlet Boundaries

Default settings (in SI) for mass-flow outlet boundary conditions are as follows:

.... Calculation Procedure at Mass-Flow Outlet Boundaries

For the Mass Flow Rate specification method, you specify the total mass flow rate,

, for the outlet.

For the Mass Flux or Mass Flux with Averaged Mass Flux specification methods, you specify the

mass flux,

(mass flow rate per unit area). If a total mass flow rate is specified, ANSYS Fluent converts

it internally to a uniform mass flux by dividing the mass flow rate by the total outlet area:

(.)

using profile files or user-defined functions. If the average mass flux is also specified, it is used to

correct the specified mass flux profile, as described previously in this section.

.

Boundary velocities are scaled to achieve the specified value of mass flow rate or mass flux. When

the mass-flow outlet is used with the profile preserving feature, a scaling factor of the specified mass

flow rate over the computed mass flow rate at the boundary is used to scale the normal face velocities

at the boundary. The other velocity components will be extrapolated from the interior. Flow variables

such as pressure, temperature, species, or other scalar quantities will be also extrapolated from adjacent

cell centers.

..... Exit Corrected Mass Flow Rate

The Exit Corrected Mass Flow Rate specification method adjusts the mass flow rate to the total

conditions at the outlet, maintaining a constant exit corrected mass flow rate. This boundary option

is mainly intended for turbomachinery applications. This method allows you to sweep through the

complete machine operational range, including machine operating points from choked flow to stall

conditions. When using the Exit Corrected Mass Flow Rate specification method, the boundary

operates like a mass-flow outlet on the left side of the speedline curve away from the best efficiency

point, and more like a pressure outlet boundary to the right of the best efficiency point all the way

beyond the choke point. This method allows you to specify the equivalent mass flow, based on

similar criteria, corrected to a specified reference temperature and pressure.

For compressible flows, the exit corrected mass flow rate (

) is calculated as:

(.)

where

and

are mass-averaged values of total pressure and temperature in the absolute frame

at the outlet.

and

are the reference conditions, which are constants in the equation. It

should be noted that the numerical behavior of the boundary condition is not affected by the choice

of reference conditions; rather, the reference conditions simply provide a dimensional meaning to

the otherwise non-dimensional mass flow rate. It is typical to specify these reference conditions to

be the same as the inflow total pressure and temperature.

In order to maintain a constant exit corrected mass flow, you can observe that the resulting mass

flow rate must be proportional to the exit total pressure and inversely proportional to the square

root of the exit total temperature (or equivalently, inversely proportional to the stagnation speed

of sound). This allows the boundary condition to adapt dynamically to varying operating conditions,

while remaining stable as the flow develops from the initial guess.

Note that the Exit Corrected Mass Flow Rate specification method is only available for ideal gas

and real gas materials.

You can obtain an initial exit corrected mass flow rate value (

) from a previously converged case

that uses standard inlet and outlet boundaries (for example, a pressure inlet and a pressure outlet).

Use the converged solution to obtain the mass-flow-averaged value of

and

at the outlet

boundary, as well as the mass flow rate (

). These values can then be applied to Equation . (p. )

along with

and

(which are usually taken as the inflow total temperature and pressure).

After you have calculated the exit corrected mass flow rate, you can adjust this value up or down

in order to traverse the speed line from choke to stall.

Inlet vent boundary conditions are used to model an inlet vent with a specified loss coefficient, flow

direction, and ambient (inlet) pressure and temperature.

.... Inputs at Inlet Vent Boundaries

You will enter the following information for an inlet vent boundary:

loss coefficient

All values are entered in the Inlet Vent Dialog Box (p. ) (Figure . : The Inlet Vent Dialog Box (p. )),

which is opened from the Boundary Conditions task page (as described in Setting Cell Zone and

The first  items listed above are specified in the same way that they are specified at pressure inlet

boundaries. See Inputs at Pressure Inlet Boundaries (p. ) for details. Specification of the loss coeffi-

cient is described here. Open channel boundary condition inputs are described in Modeling Open

Channel Flows (p. ).

Figure . : The Inlet Vent Dialog Box

..... Specifying the Loss Coefficient

An inlet vent is considered to be infinitely thin, and the pressure drop through the vent is assumed

to be proportional to the dynamic head of the fluid, with an empirically determined loss coefficient

that you supply. That is, the pressure drop,

, varies with the normal component of velocity through

the vent,

, as follows:

(.)

where  is the fluid density, and

is the non-dimensional loss coefficient.

Important

is the pressure drop in the direction of the flow; therefore the vent will appear as a

resistance even in the case of backflow.

You can define the Loss-Coefficient across the vent as a constant, polynomial, piecewise-linear,

or piecewise-polynomial function of the normal velocity. The dialog boxes for defining these

functions are the same as those used for defining temperature-dependent properties. See Defining

Properties Using Temperature-Dependent Functions (p. ) for details.

Intake fan boundary conditions are used to model an external intake fan with a specified pressure

jump, flow direction, and ambient (intake) pressure and temperature.

Note

The intake fan boundary condition considers only momentum. Diffusion processes are not

.... Inputs at Intake Fan Boundaries

You will enter the following information for an intake fan boundary:

pressure jump

All values are entered in the Intake Fan Dialog Box (p. ) (shown in Figure . : The Intake Fan Dialog

Zone and Boundary Conditions (p. )).

boundaries. See Inputs at Pressure Inlet Boundaries (p. ) for details. Specification of the pressure

jump is described here. Open channel boundary condition inputs are described in Modeling Open

Figure . : The Intake Fan Dialog Box

..... Specifying the Pressure Jump

An intake fan is considered to be infinitely thin, and the discontinuous pressure rise across it is

specified as a function of the velocity through the fan. In the case of reversed flow, the fan is treated

like an outlet vent with a loss coefficient of unity.

You can define the Pressure-Jump across the fan as a constant, polynomial, piecewise-linear, or

piecewise-polynomial function of the normal velocity. The dialog boxes for defining these functions

are the same as those used for defining temperature-dependent properties. See Defining Properties

Using Temperature-Dependent Functions (p. ) for details.

Pressure outlet boundary conditions require the specification of a static (gauge) pressure at the outlet

boundary. The value of the specified static pressure is used only while the flow is subsonic. Should

the flow become locally supersonic, the specified pressure will no longer be used; pressure will be

extrapolated from the flow in the interior. All other flow quantities are extrapolated from the interior.

A set of “backflow” conditions is also specified should the flow reverse direction at the pressure outlet

boundary during the solution process. Convergence difficulties will be minimized if you specify realistic

values for the backflow quantities.

Several options in ANSYS Fluent exist, where a radial equilibrium outlet boundary condition can be

used (see Defining Static Pressure (p. ) and a target mass flow rate for pressure outlets (see Target

Mass Flow Rate Option (p. ) for details) can be specified.

.... Inputs at Pressure Outlet Boundaries

You will enter or select the following information for a pressure outlet boundary:

pressure profile multiplier

backflow conditions

– total (stagnation) temperature (for energy calculations)

– backflow pressure specification

– backflow direction specification method

– turbulence parameters (for turbulent calculations)

– chemical species mass or mole fractions (for species calculations)

– mixture fraction and variance (for non-premixed or partially premixed combustion calculations)

– progress variable (for premixed or partially premixed combustion calculations)

– multiphase boundary conditions (for general multiphase calculations)

– type of backflow reference frame (not available for multiphase flows or with the acoustic wave model)

radial equilibrium pressure distribution

average pressure specification (not available for multiphase flows)

target mass flow rate (not available for multiphase flows)

All values are entered in the Pressure Outlet Dialog Box (p. ) (Figure . : The Pressure Outlet

Figure . : The Pressure Outlet Dialog Box

To set the static pressure at the pressure outlet boundary, enter the appropriate value for Gauge

Pressure in the Pressure Outlet dialog box. This value will be used when the flow is locally subsonic.

Should the flow become locally supersonic, the pressure will be extrapolated from the upstream

conditions. By default the subsonic and supersonic local flow condition at the boundary is determined

based on the local normal velocity component.

Operating Conditions Dialog Box (p. ). Refer to Pressure Inputs and Hydrostatic Head (p. ) re-

garding hydrostatic pressure.

ANSYS Fluent also provides an option to use a radial equilibrium outlet boundary condition. This

option is used to model the exit flow in turbomachinery flow problems. To turn on this option, enable

Radial Equilibrium Pressure Distribution. When this feature is active, the specified gauge pressure

applies only to the position of minimum radius (relative to the axis of rotation) at the boundary. The

static pressure on the rest of the zone is calculated from the assumption that radial velocity is neg-

ligible, so that the pressure gradient is given by

(.)

where  is the distance from the axis of rotation and

is the tangential velocity. Note that this

boundary condition can be used even if the rotational velocity is zero. For example, it could be applied

to the calculation of the flow through an annulus containing guide vanes.

Important

Note that the radial equilibrium outlet condition is available only for 3D and axisymmetric

swirl calculations.

ANSYS Fluent also provides an option to use an Average Pressure Specification method at the

pressure outlet boundary. This option allows the pressure along the outlet boundary to vary, but

maintain an average equivalent to the specified value in the Gauge Pressure input field. The pressure

variation allowed in this boundary implementation slightly diminishes the reflectivity of the boundary

as compared with the default uniform pressure specification. In the density-based solver two averaging

methods are available, Strong Averaging and Weak Averaging. The average pressure specification

in the pressure-based solver is the same as the strong pressure averaging in the density-based

solver. For more details, see Calculation Procedure at Pressure Outlet Boundaries (p. ).

The Pressure Profile Multiplier allows you to specify a constant factor by which the Gauge Pressure

is multiplied. This is provided mainly for cases where a non-uniform distribution of the static pressure

at the pressure outlet boundary is specified by means of a profile file or a user-defined function. The

scaling of an outlet profile with a multiplier can be convenient, for example, when computing a

performance map for a turbomachine at different mass flow rates. The option will also work for a

constant Gauge Pressure simply by scaling its value by a factor. This scaled pressure value will be

used consistently when additional options are enabled in the Pressure Outlet dialog box; for example,

when the Radial Equilibrium Pressure Distribution option is enabled, the scaled gauge pressure

will be applied to the position of minimum radius (relative to the axis of rotation) at the boundary.

..... Defining Backflow Conditions

Backflow properties consistent with the models you are using will appear in the Pressure Outlet

dialog box. The specified values will be used only if flow is pulled in through the outlet.

The Backflow Total Temperature (in the Thermal tab) should be set for problems involving energy

When the direction of the backflow re-entering the computational domain is known, and deemed to be

relevant to the flow field solution, you can specify it choosing one of the options available in the Backflow

Direction Specification Method drop-down list.The default value for this field is Normal to Boundary,

and requires no further input. If you choose Direction Vector, the dialog box will expand to show the

inputs for the components of the direction vector for the backflow, and if you are running the 3D version

of ANSYS Fluent, the dialog box will display a Coordinate System drop-down list. If you choose From

Neighboring Cell, ANSYS Fluent will determine the direction of the backflow using the direction of the

flow in the cell layer adjacent to the pressure outlet.

Instructions for deciding which method to use in determining appropriate values for these inputs are

provided in Determining Turbulence Parameters (p. ).Turbulence modeling in general is described

in Modeling Turbulence (p. ).

If you are modeling species transport, you will set the backflow species mass or mole fractions under

Species Mass Fractions or Species Mole Fractions. For details, see Defining Cell Zone and Boundary

Conditions for Species (p. ).

If you are modeling combustion using the non-premixed or partially premixed combustion model, you

will set the backflow mixture fraction and variance values. See Defining Non-Premixed Boundary Condi-

tions (p. ) for details.

If you are modeling combustion using the premixed or partially premixed combustion model, you will

set the backflow Progress Variable value. See Setting Boundary Conditions for the Progress Vari-

able (p. ) for details.

If you are using the VOF, mixture, or Eulerian model for multiphase flow, you will need to specify volume

fractions for secondary phases and (for some models) additional parameters. See Defining Multiphase

Cell Zone and Boundary Conditions (p. ) for details.

If backflow occurs,

.

The pressure you specified as the Gauge Pressure will be used to determine the total pressure or

the static pressure (based on your selection from the Backflow Pressure Specification drop-down

list), so you need not specify a backflow pressure value explicitly.When Total Pressure is selected

for Backflow Pressure Specification, boundary face pressure values are calculated by combining

the Gauge Pressure with a dynamic contribution that is based on the velocity in the adjacent cell

zone; when Static Pressure is selected for Backflow Pressure Specification, the specified Gauge

Pressure value is directly imposed as the boundary face pressure.

.

The flow direction will be based on your selection from the Backflow Direction Specification

Method drop-down list.

.

The total temperature, total pressure, and flow directions are in absolute or relative to the adjacent

cell zone reference frames, based on the Backflow Reference Frame setting specified in the Pressure

Outlet dialog box.

If the cell zone adjacent to the pressure outlet is moving (that is, if you are using a moving reference

frame, multiple reference frames, mixing planes, or sliding meshes) and you are using the pressure-

based solver, the velocity in the dynamic contribution to total pressure (see Equation . (p. ))

will be absolute or relative to the motion of the cell zone, depending on whether or not the Ab-

solute velocity formulation is selected in the General task page. For the density-based solver, the

velocity in Equation . (p. ) (or the Mach number in Equation . (p. )) is always in the

absolute frame.

Important

Even if no backflow is expected in the converged solution, you should always set realistic

values to minimize convergence difficulties in the event that backflow does occur during

the calculation.

The Backflow Reference Frame option is not available for all multiphase models or non-

reflecting boundary condition options.

flow back into the domain. The artificial walls are removed when the flow is no longer entering the

domain and when a favorable pressure gradient is recovered at the boundary mesh faces.

Note

Note

Emissivity and (optional) External Black Body Temperature Method. See Defining Boundary

Conditions for Radiation (p. ) for details. (The Rosseland radiation model does not require any

boundary condition inputs.)

pressure outlet. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

.... Default Settings at Pressure Outlet Boundaries

Default settings (in SI) for pressure outlet boundary conditions are as follows:

Gauge Pressure

Pressure Profile Multiplier

Backflow Total Temperature

%

Backflow Turbulent Intensity

Backflow Turbulent Viscosity Ratio

.... Calculation Procedure at Pressure Outlet Boundaries

At pressure outlets, if the flow exiting the boundary is subsonic, then ANSYS Fluent uses the pressure

specified in the Pressure Outlet dialog box as the static pressure of the fluid at the outlet plane,

,

and extrapolates all other conditions from the interior of the domain. However, if the flow exiting

the boundary becomes supersonic, then the face pressure values are extrapolated from the interior

cell pressure.

..... Average Pressure Specification

When this option is selected, the exit pressure is not kept constant over the pressure outlet boundary,

but instead is allowed to vary across the boundary while maintaining an average boundary pressure

close to the specified static exit pressure. This option can be used for pressure specified as a constant

or as a profile (for example, in turbomachinery cases with radial, axial, or radial equilibrium pressure

distributions).

There are two implementations of the Average Pressure Specification. These are Strong Averaging

and Weak Averaging. The strong averaging approach is available in both the density-based and

the pressure-based solver. The weak averaging approach is available only in the density-based

solver.

Note

The Average Pressure Specification option is not available with multiphase flows.

When using the density-based solver, Strong Averaging is the recommended method and

is used by default.The weak averaging method is maintained primarily for legacy cases.

When one of the Acoustic Wave Models is active, the Average Pressure Specification option

is not offered because the pressure will be obtained based on the Acoustic Wave Model

chosen.

Using the Average Pressure Specification option in unsteady simulations can result in non-

physical pressure feedback and is not recommended.

...... Strong Averaging

In the Strong Averaging approach, the face pressure value

for subsonic exit flow is computed

using the following expression:

(.)

= interior cell pressure at neighboring exit face, f

where

= averaged interior cell pressure at a boundary

= specified exit pressure

(.)

where

= pressure blending factor;

recovers the fully averaged pressure,

recovers the specified pressure.

When the strong averaging option is used with a profile specification method (radial, axial, or radial

equilibrium pressure distribution) then the outlet boundary will be subdivided into radial or axial

containers called “bins”, and the above averaging procedure is applied to each bin.

You can use the following TUI command to change the blending factor and the number of bins:

/define/boundary-conditions/bc-settings/pressure-outlet

......Weak Averaging

When the weak averaging method is used and the flow is subsonic, the pressure at the faces of the

outlet boundary is computed using a weighted average of the left and right state of the face

boundary. This weighting is a blend of fifth-order polynomials based on the exit face normal Mach

number [] (p. ). Therefore, the face pressure

is a function of (

,

,

), where

is the

interior cell pressure neighboring the exit face f,

is the specified exit pressure, and

is the face

normal Mach number.

Figure . : Pressures at the Face of a Pressure Outlet Boundary

For incompressible flows, the face pressure is computed as an average between the specified pressure

and the interior pressure.

(.)

In this boundary implementation, the exit pressure is not constant along the pressure outlet

boundary. However, upon flow convergence, the average boundary pressure will be close to the

specified static exit pressure.

.... Other Optional Inputs at Pressure Outlet Boundaries

..... Non-Reflecting Boundary Conditions Option

One of the options that may be used at pressure outlets is non-reflecting boundary conditions (NRBC).

This option is used when waves are made to pass through the boundaries while avoiding false re-

flections. Details of non-reflecting boundary conditions can be found in General Non-Reflecting

Boundary Conditions (p. ).

.....Target Mass Flow Rate Option

The simple Bernoulli's equation is used to adjust the pressure at every iteration on a pressure outlet

zone in order to meet the desired mass flow rate. The change in pressure, based on Bernoulli’s

equation is given by the following equation:

(.)

where

is the change in pressure,

is the current computed mass flow rate at the pressure-outlet

boundary,

is the required mass flow rate,

is the computed average density at the pressure-

outlet boundary, and  is the area of the pressure-outlet boundary.

Limitations

The target mass flow rate option is not available with multiphase flows or when any of the non-reflecting

boundary conditions models are used.

If the pressure-outlet zone is used in the mixing-plane model, the target mass flow rate option will not

be available for that particular zone.

The pressure outlet will not achieve the target mass flow rate if the flow becomes choked (that is, the

Mach number of the fluid in the pressure-outlet zone becomes equal to ).

The pressure outlet may not achieve the target mass flow rate if porous zones are present in the flow

domain causing a large pressure drop.

Target Mass Flow Rate Settings

To use the target mass flow rate option

. Enable Target Mass Flow Rate in the Pressure Outlet dialog box.

. Specify the Target Mass Flow as either a constant value or hook a UDF to set the target mass flow rate.

The settings for the target mass flow rate option can be accessed from the target-mass-

flow-rate-settings text command:

define → boundary-conditions → target-mass-flow-rate-settings

You will be prompted to

a.

Set the under-relaxation factor (the default setting is . ).

b. Enable the targeted mass flow rate verbosity (the default is no). If enabled, it prints to the console

window the required mass flow rate, computed mass flow rate, mean pressure, the new pressure

imposed on the outlet, and the change in pressure in SI units.

. In the Pressure Outlet dialog box, specify the Upper Limit of Absolute Pressure and Lower Limit of

Absolute Pressure. Specifying the range of the pressure limits improves convergence in cases with a

large number of outlet boundaries, which have different pressure variations on different boundaries.

You can also use the define/boundary-conditions/pressure-outlet text command to

specify these limits.

Figure . : The Pressure Outlet Dialog Box with the Target Mass Flow Rate Option Enabled

Solution Strategies When Using the Target Mass Flow Rate Option

If convergence difficulties are encountered or if the solution is not converging at the desired mass

flow rate, then try to lower the under-relaxation factor from the default value. Otherwise, you can

use the alternate method to converge at the required mass flow rate.

In some cases, you may want to switch off the target mass flow rate option initially, then guess an

exit pressure that will bring the solution closer to the target mass flow rate. After the solution stabil-

izes, you can turn on the target mass flow rate option and iterate to convergence. For many complex

flow problems, this strategy is usually very successful.

The use of Full Multigrid Initialization is also very helpful in obtaining a good starting solution and

in general will reduce the time required to get a converged solution on a target mass flow rate. For

further information on Full Multigrid Initialization, see Full Multigrid (FMG) Initialization (p. ).

Setting Target Mass Flow Rates Using UDFs

For some unsteady problems it is desirable that the target mass flow rate be a function of the

physical flow time. This enforcement of boundary condition can be done by attaching a UDF with

DEFINE_PROFILE functions to the target mass flow rate field.

Important

Note that the mass flow rate profile is a function of time and only one constant value

should be applied to all zone faces at a given time.

An example of a simple UDF using a DEFINE_PROFILE that will adjust the mass flow rate can be

found in DEFINE_PROFILE in the Fluent Customization Manual.

Pressure far-field conditions are used in ANSYS Fluent to model a free-stream condition at infinity, with

free-stream Mach number and static conditions being specified. The pressure far-field boundary con-

dition is often called a characteristic boundary condition, since it uses characteristic information

(Riemann invariants) to determine the flow variables at the boundaries.

Note the following limitations and restrictions when using pressure far-field boundary conditions:

This boundary condition is applicable only when the density is calculated using the ideal-gas law (see

Density (p. )). Using it for other flows is not permitted.To effectively approximate true infinite-extent

conditions, you must place the far-field boundary far enough from the object of interest. For example, in

lifting airfoil calculations, it is not uncommon for the far-field boundary to be a circle with a radius of

chord lengths.

It is incompatible with the multiphase models (VOF, mixture, and Eulerian) that are available with the

pressure-based solver.

It cannot be applied to flows that employ constant density, the real gas model, and the wet steam model,

which are available in the density-based solver.

.... Inputs at Pressure Far-Field Boundaries

You will enter the following information for a pressure far-field boundary:

Mach number

All values are entered in the Pressure Far-Field Dialog Box (p. ) (Figure . : The Pressure Far-Field

Figure . : The Pressure Far-Field Dialog Box

..... Defining Static Pressure, Mach Number, and Static Temperature

To set the static pressure and temperature at the far-field boundary in the Pressure Far-Field dialog

box, enter the appropriate values for Gauge Pressure and Mach Number in the Momentum tab.

The Mach number can be subsonic, sonic, or supersonic. Set the Temperature in the Thermal tab.

You can define the flow direction at a pressure far-field boundary by setting the components of the

direction vector. If your geometry is 2D non-axisymmetric enter appropriate values for X and Y in

the Pressure Far-Field dialog box (Figure . : The Pressure Far-Field Dialog Box (p. )). If your

geometry is 2D axisymmetric, enter the appropriate values for Axial, Radial, and (if you are modeling

axisymmetric swirl) Tangential-Component of Flow Direction.

If your geometry is 3D, you can choose a Coordinate System that is Cartesian, Cylindrical, or

Local Cylindrical. In the Cartesian coordinate system, enter the appropriate values for X, Y, and Z-

Component of Flow Direction. If the direction cosine data on the boundary is available, then use

the cylindrical or local cylindrical coordinate system and specify the Axial, Radial, Tangential-

Component of Flow Direction. For Cylindrical, axis parameters need to be specified on the adjacent

cell zone of the boundary face. For Local Cylindrical Swirl, specify the Axis Origin and Axis Direction.

Emissivity and (optionally) External Black Body Temperature Method. See Defining Boundary

Conditions for Radiation (p. ) for details.

..... Defining Species Transport Parameters

Mass Fractions or Species Mole Fractions. See Defining Cell Zone and Boundary Conditions for

Species (p. ) for details.

.... Defining Discrete Phase Boundary Conditions

pressure far-field boundary. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

.... Default Settings at Pressure Far-Field Boundaries

Default settings (in SI) for pressure far-field boundary conditions are as follows:

.

%

.

%

.... Calculation Procedure at Pressure Far-Field Boundaries

The pressure far-field boundary condition is a non-reflecting boundary condition based on the intro-

duction of Riemann invariants (that is, characteristic variables) for a one-dimensional flow normal to

the boundary. For flow that is subsonic there are two Riemann invariants, corresponding to incoming

and outgoing waves:

(.)

(.)

where

is the velocity magnitude normal to the boundary,  is the local speed of sound and  is

the ratio of specific heats (ideal gas). The subscript

refers to conditions being applied at infinity

(the boundary conditions), and the subscript  refers to conditions in the interior of the domain (that

is, in the cell adjacent to the boundary face). These two invariants can be added and subtracted to

give the following two equations:

(.)

(.)

where

and  become the values of normal velocity and sound speed applied on the boundary. At

a face through which flow exits, the tangential velocity components and entropy are extrapolated

from the interior; at an inflow face, these are specified as having free-stream values. Using the values

for

, , tangential velocity components, and entropy the values of density, velocity, temperature,

and pressure at the boundary face can be calculated.

Outflow boundary conditions in ANSYS Fluent are used to model flow exits where the details of the

flow velocity and pressure are not known prior to solving the flow problem. You do not define any

conditions at outflow boundaries (unless you are modeling radiative heat transfer, a discrete phase of

particles, or split mass flow): ANSYS Fluent extrapolates the required information from the interior. It

is important, however, to understand the limitations of this boundary type.

Important

Note that outflow boundaries cannot be used in the following cases:

If a problem includes pressure inlet boundaries; use pressure outlet boundary conditions (see

Pressure Outlet Boundary Conditions (p. )) instead.

If you are modeling compressible flow.

If you are modeling unsteady flows with varying density (even if the fluid is incompressible), it

is preferable to use a pressure outlet.

In general, an outflow condition may be used in incompressible cases using the Eulerian or

Mixture multiphase models. However, if the flow may produce a recirculation at the outlet

or if the flow field is not stable and fully developed at the outlet, then a pressure outlet

boundary condition is preferred.

.... ANSYS Fluent’s Treatment at Outflow Boundaries

The boundary conditions used by ANSYS Fluent at outflow boundaries are as follows:

A zero diffusion flux for all flow variables.

An overall mass balance correction.

The zero diffusion flux condition applied at outflow cells means that the conditions of the outflow

plane are extrapolated from within the domain and have no impact on the upstream flow. The extra-

polation procedure used by ANSYS Fluent updates the outflow velocity and pressure in a manner

that is consistent with a fully-developed flow assumption, as noted below, when there is no area

change at the outflow boundary.

The zero diffusion flux condition applied by ANSYS Fluent at outflow boundaries is approached

physically in fully-developed flows. Fully-developed flows are flows in which the flow velocity profile

(and/or profiles of other properties such as temperature) is unchanging in the flow direction.

It is important to note that gradients in the cross-stream direction may exist at an outflow boundary.

Only the diffusion fluxes in the direction normal to the exit plane are assumed to be zero.

.... Using Outflow Boundaries

As noted in ANSYS Fluent’s Treatment at Outflow Boundaries (p. ), the outflow boundary condition

is obeyed in fully-developed flows where the diffusion flux for all flow variables in the exit direction

are zero. However, you may also define outflow boundaries at physical boundaries where the flow is

not fully developed—and you can do so with confidence if the assumption of a zero diffusion flux at

the exit is expected to have a small impact on your flow solution. The appropriate placement of an

outflow boundary is described by example below.

Outflow boundaries where normal gradients are negligible: Figure . : Choice of the Outflow Boundary

Condition Location (p. ) shows a simple two-dimensional flow problem and several possible outflow

boundary location choices. Location C shows the outflow boundary located upstream of the plenum exit

but in a region of the duct where the flow is fully-developed. At this location, the outflow boundary con-

dition is exactly obeyed.

Figure . : Choice of the Outflow Boundary Condition Location

Ill-posed outflow boundaries: Location B in Figure . : Choice of the Outflow Boundary Condition Loca-

tion (p. ) shows the outflow boundary near the reattachment point of the recirculation in the wake of

the backward-facing step.This choice of outflow boundary condition is ill-posed as the gradients normal

to the exit plane are quite large at this point and can be expected to have a significant impact on the flow

field upstream. Because the outflow boundary condition ignores these axial gradients in the flow, location

B is a poor choice for an outflow boundary.The exit location should be moved downstream from the

reattachment point.

Figure . : Choice of the Outflow Boundary Condition Location (p. ) shows a second ill-posed

outflow boundary at location A. Here, the outflow is located where flow is pulled into the ANSYS

Fluent domain through the outflow boundary. In situations like this the ANSYS Fluent calculation

typically does not converge and the results of the calculation have no validity. This is because when

flow is pulled into the domain through an outflow, the mass flow rate through the domain is

“floating” or undefined. In addition, when flow enters the domain through an outflow boundary,

the scalar properties of the flow are not defined. For example, the temperature of the flow pulled

in through the outflow is not defined. (ANSYS Fluent chooses the temperature using the temperature

of the fluid adjacent to the outflow, inside the domain.) Therefore you should view all calculations

that involve flow entering the domain through an outflow boundary with skepticism. For such

calculations, pressure outlet boundary conditions (see Pressure Outlet Boundary Conditions (p. ))

are recommended.

Important

Note that convergence may be affected if there is recirculation through the outflow

boundary at any point during the calculation, even if the final solution is not expected

to have any flow reentering the domain. This is particularly true of turbulent flow simu-

lations.

.... Mass Flow Split Boundary Conditions

In ANSYS Fluent, it is possible to use multiple outflow boundaries and specify the fractional flow rate

through each boundary. In the Outflow Dialog Box (p. ), set the Flow Rate Weighting to indicate

what portion of the outflow is through the boundary.

Figure . : The Outflow Dialog Box

The Flow Rate Weighting is a weighting factor:

(.)

By default, the Flow Rate Weighting for all outflow boundaries is set to . If the flow is divided

equally among all of your outflow boundaries (or if you have just one outflow boundary), you need

not change the settings from the default; ANSYS Fluent will scale the flow rate fractions to obtain

equal fractions through all outflow boundaries. Therefore, if you have two outflow boundaries and

you want half of the flow to exit through each one, no inputs are required from you. If, however, you

want % of the flow to exit through one, and % through the other, you will need to explicitly

specify both Flow Rate Weighting values, that is, . for one boundary and . for the other.

Important

If you specify a Flow Rate Weighting of . at the first exit and leave the default Flow

Rate Weighting (.) at the second exit, then the flow through each boundary will be

Boundary  =

= . or .%

Boundary  =

= . or .%

.... Other Inputs at Outflow Boundaries

..... Radiation Inputs at Outflow Boundaries

In general, there are no boundary conditions for you to set at an outflow boundary. If, however, you

are using the P-, DTRM, DO, surface-to-surface, or MC models, you will set the Internal Emissivity

and (optionally) External Black Body Temperature Method in the Outflow dialog box. These

parameters are described in Defining Boundary Conditions for Radiation (p. ). The default value

for Internal Emissivity is  and the default value for Black Body Temperature is .

outflow boundary. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

ambient (discharge) pressure and temperature.

.... Inputs at Outlet Vent Boundaries

You will enter the following information for an outlet vent boundary:

– type of backflow reference frame (not available for multiphase flows)

All values are entered in the Outlet Vent Dialog Box (p. ) (Figure . : The Outlet Vent Dialog

The first  items listed above are specified in the same way that they are specified at pressure outlet

boundaries. See Inputs at Pressure Outlet Boundaries (p. ) for details. Specification of the loss

coefficient is described here. Open channel boundary condition inputs are described in Modeling

Open Channel Flows (p. ).

Figure . : The Outlet Vent Dialog Box

An outlet vent is considered to be infinitely thin, and the pressure drop through the vent is assumed

the vent,

(.)

is the nondimensional loss coefficient.

Important

You can define a constant, polynomial, piecewise-linear, or piecewise-polynomial function for

the Loss Coefficient across the vent. The dialog boxes for defining these functions are the same as

those used for defining temperature-dependent properties. See Defining Properties Using Temper-

ature-Dependent Functions (p. ) for details.

Exhaust fan boundary conditions are used to model an external exhaust fan with a specified pressure

jump and ambient (discharge) pressure.

Note

The exhaust fan boundary condition considers only momentum. Diffusion processes

are not considered.

.... Inputs at Exhaust Fan Boundaries

You will enter the following information for an exhaust fan boundary:

– user-defined scalar boundary conditions (for user-defined scalar calculations)

All values are entered in the Exhaust Fan Dialog Box (p. ) (Figure . : The Exhaust Fan Dialog

boundaries. See Inputs at Pressure Outlet Boundaries (p. ) for details. Specification of the pressure

An exhaust fan is considered to be infinitely thin, and the discontinuous pressure rise across it is

specified as a function of the local fluid velocity normal to the fan. You can define a constant,

polynomial, piecewise-linear, or piecewise-polynomial function for the Pressure Jump across the

fan. The dialog boxes for defining these functions are the same as those used for defining temper-

ature-dependent properties. See Defining Properties Using Temperature-Dependent Functions (p. )

Figure . : The Exhaust Fan Dialog Box

Important

You must be careful to model the exhaust fan so that a pressure rise occurs for forward

flow through the fan. In the case of reversed flow, the fan is treated like an inlet vent

with a loss coefficient of unity.

Degassing boundary conditions are used to model a free surface through which dispersed gas bubbles

are allowed to escape, but the continuous phase is not. A typical application is a bubble column in

which you want to reduce computational cost by not including the freeboard region in the simulation.

When the degassing boundary condition is specified for an outlet, the continuous liquid phase sees

the boundary as a free-slip wall and does not leave the domain. The dispersed gas phase sees the

boundary as an outlet. The outlet pressure is not specified. Instead, ANSYS Fluent automatically specifies

a mass sink for the dispersed gas phase in the cells adjacent to the degassing outlet. The mass sink is

calculated using the flux normal to the boundary at the cell center.

Note

The degassing boundary condition is only available for two-phase liquid-gas flows using

the Eulerian multiphase model.

The following limitations apply to the degassing boundary condition in ANSYS Fluent:

The degassing boundary condition is only available for liquid-gas two-phase flow using the Eulerian

model.The primary phase must be liquid.

In order for the gas to escape from the degassing boundary, gravity must be switched on in the model.

The degassing boundary condition is only recommended for modeling situations like bubble columns

without the freeboard region.

When postprocessing on a degassing boundary, there is no normal velocity for either phase since the gas

escape is modeled by a mass sink in the neighboring cells.

.... Inputs at Degassing Boundaries

No inputs are necessary for the degassing boundary condition. However, the initial condition for

volume fraction must be set appropriately. It is recommended that the gas phase volume fraction be

initialized with a nonzero value smaller than the steady-state gas holdup value.

Wall boundary conditions are used to bound fluid and solid regions. In viscous flows, the no-slip

boundary condition is enforced at walls by default, but you can specify a tangential velocity component

in terms of the translational or rotational motion of the wall boundary, or model a “slip” wall by spe-

cifying shear. (You can also model a slip wall with zero shear using the symmetry boundary type, but

using a symmetry boundary will apply symmetry conditions for all equations. See Symmetry Boundary

Conditions (p. ) for details.)

The shear stress and heat transfer between the fluid and wall are computed based on the flow details

in the local flow field.

.... Inputs at Wall Boundaries

You will enter the following information for a wall boundary:

wall motion conditions (for moving or rotating walls)

shear conditions (for slip walls, optional)

wall roughness (for turbulent flows, optional)

thermal boundary conditions (for heat transfer calculations)

species boundary conditions (for species calculations)

chemical reaction boundary conditions (for surface reactions)

radiation boundary conditions (for calculations using the P-, DTRM, DO, surface-to-surface, or MC

models)

wall adhesion contact angle (for VOF calculations, optional)

displacement boundary conditions for intrinsic fluid-structure interaction (FSI) simulations

....Wall Motion

Wall boundaries can be either stationary or moving. The stationary boundary condition specifies a

fixed wall, whereas the moving boundary condition can be used to specify the translational or rota-

tional velocity of the wall, or the velocity components.

Wall motion conditions are entered in the Momentum tab of the Wall Dialog Box (p. ) (Fig-

ure . : The Wall Dialog Box for a Moving Wall (p. )), which is opened from the Boundary Conditions

Task Page (p. ) (as described in Setting Cell Zone and Boundary Conditions (p. )). To view the

wall motion conditions, click the Momentum tab.

Figure . : The Wall Dialog Box for a Moving Wall

..... Defining a Stationary Wall

For a stationary wall, choose the Stationary Wall option under Wall Motion.

.....Velocity Conditions for Moving Walls

If you want to include tangential motion of the wall in your calculation, you need to define the

translational or rotational velocity, or the velocity components. Select the Moving Wall option under

Wall Motion. The Wall dialog box will expand, as shown in Figure . : The Wall Dialog Box for a

Moving Wall (p. ), to show the wall velocity conditions.

Note that you cannot use the moving wall condition to model problems where the wall motion with

respect to the adjacent cell zone has a component that is normal to the wall itself. For such problems,

consider using a Sliding or Dynamic Mesh approach as discussed in Modeling Flows Using Sliding

and Dynamic Meshes (p. ). ANSYS Fluent will neglect any normal component of wall motion that

you specify using the methods below.

Specifying Relative or Absolute Velocity

If the cell zone adjacent to the wall is moving (for example, if you are using a moving reference

frame or a sliding mesh), you can choose to specify velocities relative to the zone motion by en-

abling the Relative to Adjacent Cell Zone option. If you choose to specify relative velocities, a

velocity of zero means that the wall is stationary in the relative frame, and therefore moving at

the speed of the adjacent cell zone in the absolute frame. If you choose to specify absolute velo-

cities (by enabling the Absolute option), a velocity of zero means that the wall is stationary in

the absolute frame, and therefore moving at the speed of the adjacent cell zone—but in the op-

posite direction—in the relative reference frame.

Important

Important

If you are using one or more moving reference frames, sliding meshes, or mixing planes,

and you want the wall to be fixed in the moving frame, it is recommended that you

specify relative velocities (the default) rather than absolute velocities. Then, if you

modify the speed of the adjacent cell zone, you will not need to make any changes to

the wall velocities, as you would if you specified absolute velocities.

Note that if the adjacent cell zone is not moving, the absolute and relative options are equivalent.

Translational Wall Motion

For problems that include linear translational motion of the wall boundary (for example, a rectan-

gular duct with a moving belt as one wall) you can enable the Translational option and specify

the wall’s Speed and Direction (X,Y,Z vector). By default, wall motion is “disabled” by the specific-

ation of Translational velocity with a Speed of zero. You can define time-varying translational

speed using a transient profile (Standard Transient Profiles (p. )) or user-defined function for

the speed of the wall.

If you need to define nonlinear translational motion, you will need to use the Components option,

described below.

Rotational Wall Motion

For problems that include rotational wall motion you can enable the Rotational option and define

the rotational Speed about a specified axis. To define the axis, set the Rotation-Axis Direction

and Rotation-Axis Origin. This axis is independent of the axis of rotation used by the adjacent

cell zone, and independent of any other wall rotation axis. For 3D problems, the axis of rotation

is the vector passing through the specified Rotation-Axis Origin and parallel to the vector from

(,,) to the (X,Y,Z) point specified under Rotation-Axis Direction. For 2D problems, you will

specify only the Rotation-Axis Origin; the axis of rotation is the -direction vector passing through

the specified point. For 2D axisymmetric problems, you will not define the axis: the rotation will

always be about the  axis, with the origin at (,). You can define time-varying rotational speed

using a transient profile (Standard Transient Profiles (p. )) profile or a user-defined function for

Note that the modeling of tangential rotational motion will be correct only if the wall bounds a

surface of revolution about the prescribed axis of rotation (for example, a circle or cylinder). Note

also that rotational motion can be specified for a wall in a stationary reference frame.

Wall Motion Based on Velocity Components

For problems that include linear or nonlinear translational motion of the wall boundary you can

enable the Components option and specify the X-Velocity, Y-Velocity, and Z-Velocity of the

wall. You can define nonlinear translational motion using a profile or a user-defined function for

the X-Velocity, Y-Velocity, and/or Z-Velocity of the wall.

Wall Motion for Two-Sided Walls

As discussed earlier in this section, when you read a mesh with a two-sided wall zone (which forms

the interface between fluid/solid regions) into ANSYS Fluent, a “shadow” zone will automatically

be created so that each side of the wall is a distinct wall zone. For two-sided walls, it is possible

to specify different motions for the wall and shadow zones, whether or not they are coupled.

Note, however, that you cannot specify motion for a wall (or shadow) that is adjacent to a solid

zone.

..... Shear Conditions at Walls

Four types of shear conditions are available:

no-slip

specified shear

specularity coefficient

Marangoni stress

The no-slip condition is the default, and it indicates that the fluid sticks to the wall and moves with

the same velocity as the wall, if it is moving. The specified shear and Marangoni stress boundary

conditions are useful in modeling situations in which the shear stress (rather than the motion of the

fluid) is known. Examples of such situations are applied shear stress, slip wall (zero shear stress), and

free surface conditions (zero shear stress or shear stress dependent on surface tension gradient).

The specified shear boundary condition allows you to specify the ,

, and  components of the

shear stress as constant values or profiles. The Marangoni stress boundary condition allows you to

specify the gradient of the surface tension with respect to the temperature at this surface. The shear

stress is calculated based on the surface gradient of the temperature and the specified surface tension

gradient. The Marangoni stress option is available only for calculations in which the energy equation

is being solved.

The specularity coefficient shear condition is specifically used in multiphase with granular flows. The

specularity coefficient is a measure of the fraction of collisions that transfer momentum to the wall

and its value ranges between zero and unity. This implementation is based on the Johnson and

Jackson [] (p. ) boundary conditions for granular flows.

Shear conditions are entered in the Momentum tab of the Wall Dialog Box (p. ), which is opened

from the Boundary Conditions Task Page (p. ) (as described in Setting Cell Zone and Boundary

Conditions (p. )).

..... No-Slip Walls

You can model a no-slip wall by selecting the No Slip option under Shear Condition. This is the

default for all walls in viscous flows.

..... Specified Shear

In addition to the no-slip wall that is the default for viscous flows, you can model a slip wall by

specifying zero or nonzero shear. For nonzero shear, the shear to be specified is the shear at the

wall by the fluid. To specify the shear, select the Specified Shear option under Shear Condition

(see Figure . : The Wall Dialog Box for Specified Shear (p. )). You can then enter ,

, and

components of shear under Shear Stress. Wall functions for turbulence are not used with the Spe-

cified Shear option.

Figure . : The Wall Dialog Box for Specified Shear

..... Specularity Coefficient

For multiphase granular flow, you can specify the specularity coefficient such that when the value

is zero, this condition is equivalent to zero shear at the wall, but when the value is near unity, there

is a significant amount of lateral momentum transfer. To specify the specularity coefficient, select

the Specularity Coefficient option under Shear Condition (see Figure . : The Wall Dialog Box

for the Specularity Coefficient (p. )) and enter the desired value in the text-entry box under

Specularity Coefficient.

Note

The specularity coefficient is not available for moving walls.

Figure . : The Wall Dialog Box for the Specularity Coefficient

..... Marangoni Stress

ANSYS Fluent can also model shear stresses caused by the variation of surface tension due to tem-

perature. The shear stress applied at the wall is given by

(.)

where

is the surface tension gradient with respect to temperature, and

is the surface

gradient. This shear stress is then applied to the momentum equation.

To model Marangoni stress for the wall, select the Marangoni Stress option under Shear Condition

(see Figure . : The Wall Dialog Box for Marangoni Stress (p. )). This option is available only for

calculations in which the energy equation is being solved. You can then enter the surface tension

gradient (

in Equation . (p. )) in the Surface Tension Gradient field. Wall functions

for turbulence are not used with the Marangoni Stress option.

Figure . : The Wall Dialog Box for Marangoni Stress

.....Wall Roughness Effects in Turbulent Wall-Bounded Flows

Fluid flows over rough surfaces are encountered in diverse situations. Examples are, among many

others, flows over the surfaces of airplanes (especially due to ice accretion), ships, turbomachinery,

heat exchangers, and piping systems, and atmospheric boundary layers over terrain of varying

roughness. Wall roughness affects drag (resistance) and heat and mass transfer on the walls.

If you are modeling a turbulent wall-bounded flow in which the wall roughness effects are considered

to be significant, you can include the wall roughness effects through the Standard Law-of-the-Wall

Modified for Roughness (p. ) law-of-the-wall modified for roughness or you can use one of the

Additional Roughness Models for Icing Simulations (p. ).

...... Standard Law-of-the-Wall Modified for Roughness

Experiments in roughened pipes and channels indicate that the mean velocity distribution near

rough walls, when plotted in the usual semi-logarithmic scale, has the same slope (

) but a dif-

ferent intercept (additive constant  in the log-law). Therefore, the law-of-the-wall for mean velocity

modified for roughness has the form

(.)

where

and

(.)

where

is a roughness function that quantifies the shift of the intercept due to roughness effects.

depends, in general, on the type (uniform sand, rivets, threads, ribs, mesh-wire, and so on) and

size of the roughness. There is no universal roughness function valid for all types of roughness. For

a sand-grain roughness and similar types of uniform roughness elements, however,

has been

found to be well-correlated with the nondimensional roughness height,

, where

is

the physical roughness height and

. Analyses of experimental data show that the

roughness function is not a single function of

, but takes different forms depending on the

, where

is

value. It has been observed that there are three distinct regimes:

hydrodynamically smooth (

)

transitional (

)

fully rough (

)

According to the data, roughness effects are negligible in the hydrodynamically smooth regime, but

become increasingly important in the transitional regime, and take full effect in the fully rough regime.

In ANSYS Fluent, the whole roughness regime is subdivided into the three regimes, and the formulas

proposed by Cebeci and Bradshaw based on Nikuradse’s data  [] (p. ) are adopted to compute

for each regime.

For the hydrodynamically smooth regime (

):

(.)

For the transitional regime (

):

(.)

where

is a roughness constant, and depends on the type of the roughness.

In the fully rough regime (

):

(.)

In the solver, given the roughness parameters,

is evaluated using the corresponding formula

(Equation . (p. ), Equation . (p. ), or Equation . (p. )). The modified law-of-the-

wall in Equation . (p. ) is then used to evaluate the shear stress at the wall and other wall

functions for the mean temperature and turbulent quantities.

represents a downward shift of the logarithmic velocity profile, as shown in the following

figure:

Figure . : Downward Shift of the Logarithmic Velocity Profile

This downward shift leads to a singularity for large roughness heights and low values of

. Depending

on the turbulence model and near wall treatment, two different approaches are used in ANSYS Fluent

in order to avoid this issue:

reducing the roughness height as

decreases

decreases

The first approach consists in redefining the roughness height based on the mesh refinement:

(.)

This ensures that as

approaches zero, so too does

. Therefore, the mesh requirement for

rough walls in this case is

, in order to maintain the full effect of the roughness on the flow.

virtually shifting the wall

The second approach is based on the observation that the viscous sublayer is fully established

only near hydraulically smooth walls. In the transitional roughness regime, the roughness elements

are slightly thicker than the viscous sublayer and start to disturb it, so that in fully rough flows,

the sublayer is destroyed and viscous effects become negligible. The following figure illustrates

the equivalent sand-grain roughness using a wall with a layer of closely packed spheres, which

have an average roughness height representing a technical roughness with peaks and valleys of

different shapes and sizes (see Schlichting and Gersten [] (p. )):

Figure . : Illustration of Equivalent Sand-Grain Roughness

It can be assumed that the roughness has a blockage effect, which is about % of its height

(note that the figure above shows a two-dimensional cut of a three-dimensional arrangement).

It is therefore sensible to virtually shift the wall to % of the height of the roughness elements.

This results in a corrected

value for the first cell center:

(.)

which gives about the correct displacement caused by the surface roughness. Thus the singularity

issue is avoided and fine meshes can be handled correctly.

(.)

The second approach (that is, virtually shifting the wall) is the default treatment for rough walls for

all two-equation turbulence models based on the

equation and for the following turbulence

models based on the -equation, when they are used with standard and scalable wall functions

(note that the use of scalable wall functions is recommended over the use of standard wall functions):

standard, RNG, and realizable -  model

Reynolds stress models

All other model combinations with rough walls (for example, the Spalart-Allmaras model) have no

special calibration on fine meshes, and therefore the first approach (reducing the roughness height

as

decreases) is used.

Note

Rough walls cannot be used together with the following model combinations:

an -equation model with enhanced wall treatment or the Menter-Lechner near-wall treatment

Note that the following are the relevant -equation models:

– all of the -  models (that is, standard, RNG, and realizable)

– the Reynolds stress model with the Linear Pressure-Strain model selected

– the detached eddy simulation (DES) model with the Realizable k-epsilon option selected

the Reynolds stress model with the Stress-Omega or Stress-BSL model selected

the transition -

model

the large eddy simulation (LES) model

Important

Prior to ANSYS Fluent , the shift described by Equation . (p. ) was not applied

when using turbulence models based on the -equation. You can recover the previous

code behavior by using the following scheme command:

(rpsetvar 'ke-rough-wall-treatment-r14? #f)

(models-changed)

....... Setting the Roughness Parameters

The roughness parameters are in the Momentum tab of the Wall Dialog Box (p. ) (see Fig-

ure . : The Wall Dialog Box for Marangoni Stress (p. )), which is opened from the Boundary

Conditions Task Page (p. ) (as described in Setting Cell Zone and Boundary Conditions (p. )).

To model the wall roughness effects, you must specify two roughness parameters: the Roughness

Height,

, and the Roughness Constant,

. The default roughness height (

) is zero, which cor-

responds to smooth walls. For the roughness to take effect, you must specify a nonzero value for

. For a uniform sand-grain roughness, the height of the sand-grain can simply be taken for

.

For a non-uniform sand-grain, however, the mean diameter (

) would be a more meaningful

roughness height. For other types of roughness, an “equivalent” sand-grain roughness height could

be used for

. The above approaches are only relevant if the height is considered constant per

surface. However, if the roughness constant or roughness height is not constant, then you can specify

a profile (see Profiles (p. )). Similarly, user-defined functions may be used to define a wall roughness

height that is not constant. For details on the format of user-defined functions, refer to the Fluent

Customization Manual.

Choosing a proper roughness constant (

) is dictated mainly by the type of the given roughness.

The default roughness constant (

) was determined so that, when used with -  turbulence

models, it reproduces Nikuradse’s resistance data for pipes roughened with tightly-packed, uniform

sand-grain roughness. You may need to adjust the roughness constant when the roughness you

want to model departs much from uniform sand-grain. For instance, there is some experimental

evidence that, for non-uniform sand-grains, ribs, and wire-mesh roughness, a higher value

(

) is more appropriate. Unfortunately, a clear guideline for choosing

for arbitrary types

of roughness is not available.

Note

The advantage of the rough wall formulation using a virtual shift of the wall (Equa-

tion . (p. )) compared to reducing the roughness height as

decreases (Equa-

tion . (p. )) is that it eliminates all restrictions with respect to mesh resolution near

the wall, and can therefore be used on arbitrarily fine meshes.

...... Additional Roughness Models for Icing Simulations

Additional roughness models are available if you have selected the Spalart-Allmaras or the SST k-

ω model in the Viscous Model dialog box. See the Steps in Using a Turbulence Model (p. ) for

more information. With one of these viscous models active, the additional roughness models will

be available on the Wall boundary condition panel on the Momentum tab under Wall Roughness

→ Roughness Models → High Roughness (Icing). A discussion of the treatment of the turbulence

models with the High Roughness (Icing) enabled is given in Treatment of the Spalart-Allmaras

Model for Icing Simulations and Treatment of the SST Model for Icing Simulations. These models are

primarily designed and tested for simulations of icing applications, however they may also be useful

for other applications in which the boundary layer is fully resolved and there is surface roughness

that is large relative to the near-wall mesh.

Note that the High Roughness (Icing) models are only valid for low-Re number turbulence, or need

fine near-wall meshes (mesh should fully resolve the boundary layer).

Figure . : The Wall Dialog Box for High Roughness (Icing) Models

You have the following options:

Specified Roughness

NASA Correlation

Shin-et-al

ICE3D Roughness File

....... Specified Roughness

The Specified Roughness option is the same as in the Standard roughness model. See Setting the

Roughness Parameters (p. ) for more details.

....... NASA Correlation

If the NASA Correlation option is selected, the surface sand-grain roughness height is computed

with an empirical NASA correlation for icing in air flows [] (p. ). The sand-grain roughness

height is computed from the product of the following coefficients:

(.)

(.)

(.)

Where

is the Free Stream Velocity,

is the Free Stream Temperature, LC is the Liquid Content

(in most cases water for ice accretion), c is the Characteristic Length, and

.

The sand-grain roughness height is then obtained from the formulation:

(.)

....... Shin-et-al

If the Shin-et-al option is selected the empirical correlation for the surface sand-grain roughness is

computed with the Shin and Bond formulation [] (p. ), which modifies the NASA correlation

(see the NASA Correlation (p. ) for a description of variables) with the following factor:

(.)

where MVD is the droplet mean diameter (Droplet Diameter). The corresponding value of the sand-

grain roughness height is obtained from:

(.)

....... ICE3D Roughness File

If the ICE3D Roughness File is selected, the sand-grain roughness height is read from a node-based

input file obtained from FENSAP-ICE. The file must have the format

, and be read in

Fluent via File → Read → Profile. After the FENSAP-ICE roughness file is read into Fluent, the file

name will appear in the dropdown list.

....Thermal Boundary Conditions at Walls

When you are solving the energy equation, you need to define thermal boundary conditions at wall

boundaries. Seven types of thermal conditions are available:

fixed heat flux

fixed temperature

convective heat transfer

external radiation heat transfer

combined external radiation and convection heat transfer

thermal data transferred between another system in Workbench using System Coupling

thermal coupling across a mapped interface

If the wall zone is a “two-sided wall” (a wall that forms the interface between two regions, such as

the fluid/solid interface for a conjugate heat transfer problem) a subset of these thermal conditions

will be available, but you will also be able to choose whether or not the two sides of the wall are

“coupled”. See below for details.

The inputs for each type of thermal condition are described below. If the wall has a nonzero-thickness,

you should also set parameters for calculating thin-wall thermal resistance and heat generation in

the wall, as described below.

You can model conduction within boundary walls and internal (that is, two-sided) walls of your

model. This type of conduction, called shell conduction, allows you to more conveniently model heat

conduction on walls where the wall thickness is small with respect to the overall geometry (for example,

finned heat exchangers or sheet metal in automobile underhoods). Meshing these walls with solid

cells would lead to high-aspect-ratio meshes and a significant increase in the total number of cells.

See below for details about shell conduction.

Thermal conditions are entered in the Thermal tab of the Wall Dialog Box (p. ) (Figure . : The

Wall Dialog Box (Thermal Tab) (p. )), which is opened from the Boundary Conditions task page

(as described in Setting Cell Zone and Boundary Conditions (p. )).

Figure . : The Wall Dialog Box (Thermal Tab)

..... Heat Flux Boundary Conditions

For a fixed heat flux condition, choose the Heat Flux option under Thermal Conditions. You will

then need to set the appropriate value for the heat flux at the wall surface in the Heat Flux field.

You can define an adiabatic wall by setting a zero heat flux condition. This is the default condition

for all walls.

.....Temperature Boundary Conditions

To select the fixed temperature condition, choose the Temperature option under Thermal Conditions

in the Wall dialog box. You will need to specify the temperature at the wall surface (Temperature).

The heat transfer to the wall is computed using Equation . (p. ) or Equation . (p. ).

..... Convective Heat Transfer Boundary Conditions

For a convective heat transfer wall boundary, select Convection under Thermal Conditions. Your

inputs of Heat Transfer Coefficient and Free Stream Temperature will allow ANSYS Fluent to

compute the heat transfer to the wall using Equation . (p. ).

..... External Radiation Boundary Conditions

If radiation heat transfer from the exterior of your model is of interest, you can enable the Radiation

option in the Wall dialog box and set the External Emissivity and External Radiation Temperature.

..... Combined Convection and External Radiation Boundary Conditions

You can choose a thermal condition that combines the convection and radiation boundary conditions

by selecting the Mixed option. With this thermal condition, you will need to set the Heat Transfer

Coefficient, Free Stream Temperature, External Emissivity, and External Radiation Temperature.

..... Augmented Heat Transfer

When modeling the heat transfer of applications that have perturbed flow and/or disturbed

boundary layers, it can be necessary to augment the calculation of the diffusive heat flux with a

convective augmentation factor. Such applications include the modeling of underhood and underbody

heat loads, as wells as transient heat transfer in fully warmed-up exhaust systems.

The convective augmentation factor represents the ratio of the measured Nusselt number to the

Nusselt number of an ideal flow. You can define it by using the following text command:

define → boundary-conditions → wall

You will be prompted to define the Convective Augmentation Factor as either a profile or

a single value. Note that a value of  (the default value) represents no augmentation of the diffusive

heat flux, whereas values greater than  initiate augmentation. For further details, see the equation

for qid in DEFINE_HEAT_FLUX of the Fluent Customization Manual.

.....Thin-Wall Thermal Resistance Parameters

By default, a wall will have a thickness of zero. You can, however, in conjunction with any of the

thermal conditions, model a thin layer of material on the wall. For example, you can model the effect

of a piece of sheet metal between two fluid zones, a coating on a solid zone, or contact resistance

between two solid regions. ANSYS Fluent will solve a 1D steady heat conduction equation to compute

the thermal resistance offered by the wall and the heat generation in the wall.

To include these effects in the heat transfer calculation you will need to specify the type of material,

the thickness of the wall, and the heat generation rate in the wall. Select the material type in the

Material Name drop-down list, and specify the thickness in the Wall Thickness field. If you want

to check or modify the properties of the selected material, you can click Edit... to open the Edit

Material dialog box; this dialog box contains just the properties of the selected material, not the

full contents of the standard Create/Edit Materials dialog box.

When you specify a thickness, the wall is then treated as a coupled wall, where the surface that is

adjacent to the fluid / solid cells is referred to as the “wall surface”. See Figure . : A Thin Wall (p. ).

Figure . : A Thin Wall

The thermal resistance of the wall is

, where  is the conductivity of the wall material and

is the wall thickness. The thermal wall boundary condition you set will be specified on the surface

that is separated from the fluid / solid cells by the wall thickness. The temperature specified at this

side of the wall is

.

Important

Note that for thin walls, you can only specify a constant thermal conductivity. If you want

to use a non-constant thermal conductivity for a wall with nonzero-thickness, you should

use the shell conduction model (see Shell Conduction (p. ) for details).

Specify the heat generation rate inside the wall in the Heat Generation Rate field. This option is

useful if, for example, you are modeling printed circuit boards where you know the electrical power

dissipated in the circuits.

When postprocessing a wall that has a thickness but does not have shell conduction enabled, the

Temperature... category provides three options: the temperature of the adjacent fluid / solid cells

are stored as Static Temperature; the temperature of the wall surface itself is stored as Wall Tem-

perature; and the temperature of the surface that is separated from the fluid / solid cells by the

wall thickness is stored as Wall Temperature (Thin). If a more detailed analysis of the solid zone

and surfaces is required, then you should consider creating layers of solid cells in your meshing ap-

plication.

.....Thermal Conditions for Two-Sided Walls

If the wall zone has a fluid or solid region on each side, it is called a “two-sided wall”. When you

read a mesh with this type of wall zone into ANSYS Fluent, a “shadow” zone will automatically be

created so that each side of the wall is a distinct wall zone. In the Wall dialog box, the shadow zone’s

name will be shown in the Shadow Face Zone field. You can choose to specify different thermal

conditions on each zone, or to couple the two zones:

To couple the two sides of the wall, select the Coupled option under Thermal Conditions. (This option

will appear in the Wall dialog box only when the wall is a two-sided wall.) No additional thermal

boundary conditions are required, because the solver will calculate heat transfer directly from the solution

in the adjacent cells.You can, however, specify the material type, wall thickness, and heat generation

rate for thin-wall thermal resistance calculations, as described above. Note that the resistance parameters

you set for one side of the wall will automatically be assigned to its shadow wall zone. Specifying the

heat generation rate inside the wall is useful if, for example, you are modeling printed circuit boards

where you know the electrical power dissipated in the circuits but not the heat flux or wall temperature.

To uncouple the two sides of the wall and specify different thermal conditions on each one, choose

Temperature or Heat Flux as the thermal condition type (Convection and Radiation are not applicable

for two-sided walls); note that this uncoupling will not be effective if you have enabled shell conduction

for the wall.The relationship between the wall and its shadow will be retained, so that you can couple

them again at a later time, if desired.You will need to set the relevant parameters for the selected thermal

condition, as described above.The two uncoupled walls can have different thicknesses, and are effectively

insulated from one another. If you specify a nonzero wall thickness for the uncoupled walls, the thermal

boundary conditions you set will be specified for each thin wall on the surface that is separated from

the fluid / solid cells by the wall thickness, as shown in Figure . : Uncoupled Thin Walls (p. ), where

is the Temperature (or

is the Heat Flux) specified on one wall and

is the Heat Flux) specified on the other wall.

and

are the thermal conductivities of the un-

coupled thin walls. Note that the gap between the walls in Figure . : Uncoupled Thin Walls (p. ) is

not part of the model; it is included in the figure only to show where the thermal boundary condition

for each uncoupled wall is applied.

Figure . : Uncoupled Thin Walls

..... Shell Conduction

To enable shell conduction for a wall, enable the Shell Conduction option in the Wall boundary

condition dialog box. You can then click the Edit... button to open the Shell Conduction Layers

dialog box, where you can define the properties of the single or multiple layers of the shell. Note

that you must specify a nonzero wall thickness for every layer of the shell. When shell conduction

is enabled, ANSYS Fluent will compute heat conduction for the wall not only in the normal direction

(which is always computed when the energy equation is solved), but also in the planar directions.

The Shell Conduction option will appear in the Wall dialog box for all walls when solution of the

energy equation is active (except for mapped interfaces). For information about how the thermal

conditions are applied on a wall with shell conduction enabled, managing multiple shells, and

postprocessing shell conduction walls, see Shell Conduction Considerations (p. ).

ANSYS Fluent cases with shell conduction can be read in serial or parallel. Either a partitioned or an

unpartitioned case file can be read in parallel (see Mesh Partitioning and Load Balancing (p. ) for

more information on partitioning). After reading a case file in parallel, shell zones can be created on

any wall.

To convert every wall with a finite thickness into a shell with a single action, the TUI command

define/boundary-conditions/modify-zones/create-all-shell-threads can be

used; each converted shell will have a single layer with the same thickness as the original thin wall

(any pre-existing shells will not be modified). To disable shell conduction in every wall with a single

action, the TUI command define/boundary-conditions/modify-zones/delete-all-

shells can be used. These capabilities are available in both serial and parallel mode.

Important

Important

Note that the shell conduction model has several limitations:

It cannot be applied on non-conformal interfaces, including mapped interfaces.

It cannot be applied on moving wall zones.

It cannot be used with FMG initialization.

Shell conduction is not available when the wall is set up to receive thermal data via System

Coupling.

It is available only in 3D.

It is available only when the pressure-based solver is used.

Shells cannot be split or merged. If you need to split or merge a shell, disable the Shell Con-

duction option for the wall, perform the split or merge operation, and then enable Shell

Conduction for the new wall zones.

The shell conduction model cannot be used on a wall zone that has undergone hanging

node adaption. If you want to perform such adaption elsewhere in the computational

domain, be sure to use a boolean operation in an adaption expression to exclude a

register containing the walls you are using for shell conduction. For example,

NOT(region_0). Refer to Adapting the Mesh (p. ) for additional information on

adapting the mesh.

Fluxes at the ends of a shell are not included in the heat balance reports.These fluxes are

accounted for correctly in the ANSYS Fluent solution, but not in the flux report itself.

The junction of a wall with shell conduction enabled and a non-conformal coupled wall is not

supported. Such a junction will not be thermally connected, that is, there will be no heat

transfer between the shell and the mesh interface wall.

When running the parallel solver with the shell conduction model, note that coupled walls

are encapsulated. If you encounter problems with the partitioning of the mesh, you can try

changing the encapsulation method to see if that resolves the problem (see Troubleshoot-

ing (p. ) for this and other troubleshooting options).

..... Heat Transfer Boundary Conditions Through System Coupling

System Coupling allows the input and output of thermal data from ANSYS Fluent. When Fluent is

coupled with another system in Workbench using System Coupling, you can select the via System

Coupling option on the desired wall boundaries to receive thermal data through System Coupling

service. Note that this option does not need to be selected to provide thermal data from Fluent.

For more details about setting up a simulation with System Coupling, see the Performing System

Coupling Simulations Using Fluent (p. ) and the System Coupling User's Guide.

When thermal data is transferred into Fluent via System Coupling, the following variables are available:

heat flow (heat rate)

When thermal data is transferred out of Fluent via System Coupling, the following variables are

available:

heat transfer coefficient (also known as “convection coefficient”)

near wall temperature (also known as “bulk temperature” or “ambient temperature”)

For each data transfer, you specify the type of data transfer (the variables transferred) during the

System Coupling setup.

As part of standard heat transfer boundary condition settings in ANSYS Fluent, you can also specify

the type of material, the thickness of the wall, and the heat generation rate in the wall. Select the

material type in the Material Name drop-down list; if you want to check or modify the properties

of the selected material, you can click Edit... to open the Edit Material dialog box (this dialog box

contains just the properties of the selected material, and not the full contents of the standard Cre-

ate/Edit Materials dialog box). You can specify the thickness in the Wall Thickness number-entry

box and the heat generation rate in the Heat Generation Rate number-entry box.

Note

A boundary will behave in the same way as an adiabatic boundary if the via System

Coupling option is enabled on this boundary, and ANSYS Fluent is not receiving data

from the coupling data transfer. Fluent is not receiving coupling data if it is either not

involved with a System Coupling simulation, or if the coupling is a one-way transfer with

the Fluent analysis only providing data to the second solver.

..... Heat Transfer Boundary Conditions Across a Mapped Interface

Mapped interfaces provide a robust approach for modeling coupled walls between zones when the

interface zones penetrate each other or have gaps between them (see Figure . : 2D Interface with

Penetration and Gaps (p. )). For the interface wall boundary zones created as part of such interfaces,

via Mapped Interface is automatically selected from the Thermal Conditions list in the Thermal

tab of the Wall dialog box, in order to interpolate the thermal data.

Important

Note that thermal coupling calculations will not be performed at mapped interfaces for

Important

For more details about mapped interfaces, see The Mapped Option (p. ) and Using a Non-Con-

formal Mesh in ANSYS Fluent (p. ).

Figure . : 2D Interface with Penetration and Gaps

Such boundaries also allow you to specify the standard heat transfer boundary condition settings,

such as the type of material, the thickness of the wall, and the heat generation rate in the wall. Select

the material type in the Material Name drop-down list; if you want to check or modify the properties

box and the heat generation rate in the Heat Generation Rate number-entry box. Note that the

Shell Conduction option is not available with the via Mapped Interface thermal condition.

.... Species Boundary Conditions for Walls

By default, a zero-gradient condition for all species is assumed at walls (except for species that parti-

cipate in surface reactions), but it is also possible to specify species mass fractions at walls. That is,

Dirichlet boundary conditions such as those that are specified at inlets can be used at walls as well.

If you want to retain the default zero-gradient condition for a species, no inputs are required. If you

want to specify the mass fraction for a species at the wall, the steps are as follows:

. Click the Species tab in the Wall Dialog Box (p. ) to view the species boundary conditions for the wall

(see Figure . :The Wall Dialog Box for Species Boundary Condition Input (p. )).

. Under Species Boundary Condition, select Specified Mass Fraction (rather than Zero Diffusive Flux)

in the drop-down list to the right of the species name.The dialog box will expand to include a field for

Species Mass Fractions.

Figure . : The Wall Dialog Box for Species Boundary Condition Input

. Under Species Mass Fractions, specify the mass fraction for the species.

The boundary condition type for each species is specified separately, so you can choose to use different

methods for different species.

If you are modeling species transport with reactions, you can, alternatively, enable a reaction mech-

anism at a wall by turning on the Reaction option and selecting an available mechanism from the

Reaction Mechanisms drop-down list. See Defining Zone-Based Reaction Mechanisms (p. ) for

more information about defining reaction mechanisms.

You can also model unresolved surface washcoats, which greatly increase the catalytic surface area,

by specifying the Surface Area Washcoat Factor. The surface washcoat increases the area available

for surface reaction.

..... Reaction Boundary Conditions for Walls

If you have enabled the modeling of wall surface reactions in the Species Model Dialog Box (p. ),

you can indicate whether or not surface reactions should be activated for the wall. In the Species

tab of the Wall dialog box (Figure . : The Wall Dialog Box for Species Boundary Condition In-

put (p. )), turn the Surface Reactions option on or off.

Note that a zero-gradient condition is assumed at the wall for species that do not participate in any

surface reactions.

.... Radiation Boundary Conditions for Walls

If you are using the gray P-, DTRM, DO, surface-to-surface, or MC models, you will need to set the

emissivity of the wall (Internal Emissivity) in the Thermal tab of the Wall dialog box. If you are using

the Rosseland model you do not need to set the emissivity, because ANSYS Fluent assumes the

emissivity is .

For the non-gray P-, DO, or MC models, specify a constant Internal Emissivity for each wavelength

band in the Radiation tab of the Wall dialog box (the default value in each band is ). Alternatively,

you can specify the internal emissivity using a boundary condition parameter (see Creating a New

Parameter (p. )). If you are using the non-gray DO or MC models, you will also need to define the

wall as opaque or semi-transparent in the Radiation tab. See Defining Boundary Conditions for Radi-

ation (p. ) for details. If you are using the DO or MC models, you can enable a Boundary Source.

.... Discrete Phase Model (DPM) Boundary Conditions for Walls

wall in the DPM section of the Wall dialog box. See Setting Boundary Conditions for the Discrete

Phase (p. ) for details.

.....Wall Adhesion Contact Angle for VOF Model

If you are using the VOF model and you are modeling wall adhesion, you can specify the contact

angle for each pair of phases at the wall in the Momentum tab of the Wall dialog box. See Steps

for Setting Boundary Conditions (p. ) for details.

.... User-Defined Scalar (UDS) Boundary Conditions for Walls

If you have defined UDS transport equations in your model, you can specify boundary conditions for

each equation in the UDS section of the Wall dialog box. See Setting Up UDS Equations in ANSYS

Fluent (p. ) for details.

....Wall Film Conditions for Walls

If you are using the Eulerian Wall Film model (see Modeling Eulerian Wall Films (p. ) for details),

you can set liquid film conditions at the wall in the Wall Film tab of the Wall dialog box. This tab is

available only if you have enabled the Eulerian Wall Film model in the Models Task Page (p. ).

For details, see Setting Eulerian Wall Film Solution Controls (p. ).

.... Structural Model Conditions for Walls

For an intrinsic fluid-structure interaction (FSI) simulation, you can set the displacement boundary

condition settings for walls that are adjacent to solid cell zones in the Structure tab of the Wall dialog

box. This tab is only available when a model is selected in the Structural Model Dialog Box (p. ).

For details, see Setting Up an Intrinsic Fluid-Structure Interaction (FSI) Simulation (p. ).

.... Default Settings at Wall Boundaries

The default thermal boundary condition is a fixed heat flux of zero. Walls are, by default, not moving.

.... Shear-Stress Calculation Procedure at Wall Boundaries

For no-slip wall conditions, ANSYS Fluent uses the properties of the flow adjacent to the wall/fluid

boundary to predict the shear stress on the fluid at the wall. In laminar flows this calculation simply

depends on the velocity gradient at the wall, while in turbulent flows one of the approaches described

in Near-Wall Treatments for Wall-Bounded Turbulent Flows in the Theory Guide is used.

For specified-shear walls, ANSYS Fluent will compute the tangential velocity at the boundary.

If you are modeling inviscid flow with ANSYS Fluent, all walls use a slip condition, so they are frictionless

and exert no shear stress on the adjacent fluid.

..... Shear-Stress Calculation in Laminar Flow

In a laminar flow, the wall shear stress is defined by the normal velocity gradient at the wall as

(.)

When there is a steep velocity gradient at the wall, you must be sure that the mesh is sufficiently

fine to accurately resolve the boundary layer. Guidelines for the appropriate placement of the near-

wall node in laminar flows are provided in Mesh Element Distribution (p. ).

..... Shear-Stress Calculation in Turbulent Flows

Wall treatments for turbulent flows are described in Near-Wall Treatments for Wall-Bounded Turbulent

Flows in the Theory Guide.

.... Heat Transfer Calculations at Wall Boundaries

When a fixed temperature condition is applied at the wall, the heat flux to the wall from a fluid cell

is computed as

(.)

where

= fluid-side local heat transfer coefficient

= wall surface temperature

= local fluid temperature

= radiative heat flux

Note that the fluid-side heat transfer coefficient is computed based on the local flow-field conditions

(for example, turbulence level, temperature, and velocity profiles), as described by Equa-

Heat transfer to the wall boundary from a solid cell is computed as

(.)

where

= thermal conductivity of the solid

= local solid temperature

= distance between wall surface and the solid cell center

When you define a heat flux boundary condition at a wall, you specify the heat flux at the wall surface.

ANSYS Fluent uses Equation . (p. ) and your input of heat flux to determine the wall surface

temperature adjacent to a fluid cell as

(.)

where, as noted above, the fluid-side heat transfer coefficient is computed based on the local flow-

field conditions. When the wall borders a solid region, the wall surface temperature is computed as

(.)

When you specify a convective heat transfer coefficient boundary condition at a wall, ANSYS Flu-

ent uses your inputs of the external heat transfer coefficient and external heat sink temperature to

compute the heat flux to the wall as

(.)

where

= external heat transfer coefficient defined by you

= external heat-sink temperature defined by you

Equation . (p. ) assumes a wall of zero-thickness.

When the external radiation boundary condition is used in ANSYS Fluent, the heat flux to the wall

(.)

where

= emissivity of the external wall surface defined by you

= Stefan-Boltzmann constant

= surface temperature of the wall

= temperature of the radiation source or sink on the exterior of the domain, defined

by you

= radiative heat flux to the wall from within the domain

by you

..... Combined External Convection and Radiation Boundary Conditions

When you choose the combined external heat transfer condition, the heat flux to the wall is computed

as

(.)

where the variables are as defined above. Equation . (p. ) assumes a wall of zero-thickness.

..... Calculation of the Fluid-Side Heat Transfer Coefficient

In laminar flows, the fluid side heat transfer at walls is computed using Fourier’s law applied at the

walls. ANSYS Fluent uses its discrete form:

(.)

where  is the local coordinate normal to the wall.

For turbulent flows, ANSYS Fluent uses the law-of-the-wall for temperature derived using the analogy

between heat and momentum transfer  [] (p. ). See Standard Wall Functions in the separate

Theory Guide for details.

Symmetry boundary conditions are used when the physical geometry of interest, and the expected

pattern of the flow/thermal solution, have mirror symmetry. They can also be used to model zero-shear

slip walls in viscous flows. This section describes the treatment of the flow at symmetry planes and

provides examples of the use of symmetry. You do not define any boundary conditions at symmetry

boundaries, but you must take care to correctly define your symmetry boundary locations.

Important

At the centerline of an axisymmetric geometry, you should use the axis boundary type

rather than the symmetry boundary type, as illustrated in Figure . : Use of an Axis

Important

Boundary as the Centerline in an Axisymmetric Geometry (p. ). See Axis Boundary Condi-

.... Examples of Symmetry Boundaries

Symmetry boundaries are used to reduce the extent of your computational model to a symmetric

subsection of the overall physical system. Figure . : Use of Symmetry to Model One Quarter of a

3D Duct (p. ) and Figure . : Use of Symmetry to Model One Quarter of a Circular Cross-Sec-

tion (p. ) illustrate two examples of symmetry boundary conditions used in this way.

Figure . : Use of Symmetry to Model One Quarter of a 3D Duct

Figure . : Use of Symmetry to Model One Quarter of a Circular Cross-Section

Figure . : Inappropriate Use of Symmetry (p. ) illustrates two problems in which a symmetry

plane would be inappropriate. In both examples, the problem geometry is symmetric but the flow itself

does not obey the symmetry boundary conditions. In the first example, buoyancy creates an asym-

metric flow. In the second, swirl in the flow creates a flow normal to the would-be symmetry plane.

Note that this second example should be handled using rotationally periodic boundaries (as illustrated

in Figure . : Use of Periodic Boundaries to Define Swirling Flow in a Cylindrical Vessel (p. )).

Figure . : Inappropriate Use of Symmetry

.... Calculation Procedure at Symmetry Boundaries

ANSYS Fluent assumes a zero flux of all quantities across a symmetry boundary. There is no convective

flux across a symmetry plane: the normal velocity component at the symmetry plane is therefore

zero. There is no diffusion flux across a symmetry plane: the normal gradients of all flow variables are

therefore zero at the symmetry plane. The symmetry boundary condition can therefore be summarized

zero normal velocity at a symmetry plane

zero normal gradients of all variables at a symmetry plane

As stated above, these conditions determine a zero flux across the symmetry plane, which is required

by the definition of symmetry. Since the shear stress is zero at a symmetry boundary, it can also be

interpreted as a “slip” wall when used in viscous flow calculations.

Periodic boundary conditions are used when the physical geometry of interest and the expected pattern

of the flow/thermal solution have a periodically repeating nature. Two types of periodic conditions

are available in ANSYS Fluent. The first type does not allow a pressure drop across the periodic planes.

(Note to FLUENT  users: This type of periodic boundary is referred to as a “cyclic” boundary in FLUENT

.) The second type allows a pressure drop to occur across translationally periodic boundaries, enabling

you to model “fully-developed” periodic flow. (In FLUENT  this is a “periodic” boundary.)

This section discusses the no-pressure-drop periodic boundary condition. A complete description of

the fully-developed periodic flow modeling capability is provided in Periodic Flows (p. ).

.... Examples of Periodic Boundaries

Periodic boundary conditions are used when the flows across two opposite planes in your computa-

tional model are identical. Figure . : Use of Periodic Boundaries to Define Swirling Flow in a Cyl-

indrical Vessel (p. ) illustrates a typical application of periodic boundary conditions. In this example

the flow entering the computational model through one periodic plane is identical to the flow exiting

the domain through the opposite periodic plane. Periodic planes are always used in pairs as illustrated

in this example.

Figure . : Use of Periodic Boundaries to Define Swirling Flow in a Cylindrical Vessel

.... Inputs for Periodic Boundaries

For a periodic boundary without any pressure drop, there is only one input you need to consider:

whether the geometry is rotationally or translationally periodic. (Additional inputs are required for a

periodic flow with a periodic pressure drop. See Periodic Flows (p. ).)

Rotationally periodic boundaries are boundaries that form an included angle about the centerline of

a rotationally symmetric geometry. Figure . : Use of Periodic Boundaries to Define Swirling Flow in

a Cylindrical Vessel (p. ) illustrates rotational periodicity. Translationally periodic boundaries are

boundaries that form periodic planes in a rectilinear geometry. Figure . : Example of Translational

Periodicity - Physical Domain (p. ) illustrates translationally periodic boundaries.

Figure . : Example of Translational Periodicity - Physical Domain

Figure . : Example of Translational Periodicity - Modeled Domain

You will specify translational or rotational periodicity for a periodic boundary in the Periodic Dialog

Box (p. ) (Figure . : The Periodic Dialog Box (p. )), which is opened from the Boundary Condi-

tions task page (as described in Setting Cell Zone and Boundary Conditions (p. )).

Figure . : The Periodic Dialog Box

Note that there will be an additional item in the Periodic dialog box for the density-based solver,

which allows you to specify the periodic pressure jump. See Periodic Flows (p. ) for details.

If the domain is rotationally periodic, select Rotational as the Periodic Type; if it is translationally

periodic, select Translational. For rotationally periodic domains, the solver will automatically compute

the angle through which the periodic zone is rotated. The axis used for this rotation is the axis of

rotation specified for the adjacent cell zone.

Note that there is no need for the adjacent cell zone to be moving for you to use a rotationally peri-

odic boundary. You could, for example, model pipe flow in 3D using a stationary reference frame

with a pie-slice of the pipe; the sides of the slice would require rotational periodicity.

Click the Check button in the Mesh group box of the  Domain tab (see Checking the Mesh (p. ))

to compute and display the minimum, maximum, and average rotational angles of all faces on peri-

odic boundaries. If the difference between the minimum, maximum, and average values is not negli-

gible, then there is a problem with the mesh: the mesh geometry is not periodic about the specified

axis.

.... Default Settings at Periodic Boundaries

By default, all periodic boundaries are translational.

axis.

.... Calculation Procedure at Periodic Boundaries

ANSYS Fluent treats the flow at a periodic boundary as though the opposing periodic plane is a direct

neighbor to the cells adjacent to the first periodic boundary. Therefore, when calculating the flow

through the periodic boundary adjacent to a fluid cell, the flow conditions at the fluid cell adjacent

to the opposite periodic plane are used.

The axis boundary type must be used as the centerline of an axisymmetric geometry (see Figure . : Use

of an Axis Boundary as the Centerline in an Axisymmetric Geometry (p. )). It can also be used for

the centerline of a cylindrical-polar quadrilateral or hexahedral mesh (for example, a mesh created for

a structured-mesh code such as FLUENT ). You do not need to define any boundary conditions at

axis boundaries.

Important

When creating 2D axisymmetric geometry, the axis boundary must lie on the y= line.

Figure . : Use of an Axis Boundary as the Centerline in an Axisymmetric Geometry

.... Calculation Procedure at Axis Boundaries

To determine the appropriate physical value for a particular variable at a point on the axis, ANSYS

Fluent uses the cell value in the adjacent cell.

The fan model is a lumped parameter model that can be used to determine the impact of a fan with

known characteristics upon some larger flow field. The fan boundary type allows you to input an em-

pirical fan curve that governs the relationship between head (pressure rise) and flow rate (velocity)

across a fan element. You can also specify radial and tangential components of the fan swirl velocity.

The fan model does not provide an accurate description of the detailed flow through the fan blades.

Instead, it predicts the amount of flow through the fan. Fans may be used in conjunction with other

flow sources, or as the sole source of flow in a simulation. In the latter case, the system flow rate is

determined by the balance between losses in the system and the fan curve.

ANSYS Fluent also provides a connection for a special user-defined fan model that updates the pressure

jump function during the calculation. This feature is described in User-Defined Fan Model (p. ).

.... Fan Equations

..... Modeling the Pressure Rise Across the Fan

A fan is considered to be infinitely thin, and the discontinuous pressure rise across it is specified as

a function of the velocity through the fan. The relationship may be a constant, a polynomial, piecewise-

linear, or piecewise-polynomial function, or a user-defined function.

In the case of a polynomial, the relationship is of the form

(.)

where

is the pressure jump,

are the pressure-jump polynomial coefficients, and  is the

magnitude of the local fluid velocity normal to the fan.

Important

The velocity  can be either positive or negative. You must be careful to model the fan

You can, optionally, use the mass-averaged velocity normal to the fan to determine a single pressure-

jump value for all faces in the fan zone.

..... Modeling the Fan Swirl Velocity

For three-dimensional problems, the values of the convected tangential and radial velocity fields

can be imposed on the fan surface to generate swirl. These velocities can be specified as functions

of the radial distance from the fan center. The relationships may be constant or polynomial functions,

or user-defined functions.

Important

You must use SI units for all fan swirl velocity inputs.

For the case of polynomial functions, the tangential and radial velocity components can be specified

by the following equations:

(.)

(.)

where

and

are, respectively, the tangential and radial velocities on the fan surface in m/s,

and

are the tangential and radial velocity polynomial coefficients, and  is the distance to the

fan center.

.... User Inputs for Fans

Once the fan zone has been identified (in the Boundary Conditions task page), you will set all

modeling inputs for the fan in the Fan Dialog Box (p. ) (Figure . : The Fan Dialog Box (p. )),

which is opened from the Boundary Conditions Task Page (p. ) (as described in Setting Cell Zone

and Boundary Conditions (p. )).

Figure . : The Fan Dialog Box

Inputs for a fan are as follows:

. Identify the fan zone.

. Define the pressure jump across the fan.

. Define the discrete phase boundary condition for the fan (for discrete phase calculations).

. Define the swirl velocity, if desired (3D only).

..... Identifying the Fan Zone

Since the fan is considered to be infinitely thin, it must be modeled as the interface between cells,

rather than a cell zone. Therefore the fan zone is a type of internal face zone (where the faces are

line segments in 2D or triangles/quadrilaterals in 3D). If, when you read your mesh into ANSYS Fluent,

the fan zone is identified as an interior zone, right-click the zone in the tree and use the Type sub-

menu to change it to a fan zone (for more details, see Changing Cell and Boundary Zone

Once the interior zone has been changed to a fan zone, you can open the Fan dialog box and specify

the pressure jump and, optionally, the swirl velocity.

..... Defining the Pressure Jump

To define the pressure jump, you will specify a polynomial, piecewise-linear, or piecewise-polynomial

function of velocity, a user-defined function, or a constant value. You should also check the Zone

Average Direction vector to be sure that a pressure rise occurs for forward flow through the fan.

The Zone Average Direction, calculated by the solver, is the face-averaged direction vector for the

fan zone. If this vector is pointing in the direction you want the fan to blow, do not select Reverse

Fan Direction; if it is pointing in the opposite direction, select Reverse Fan Direction.

...... Polynomial, Piecewise-Linear, or Piecewise-Polynomial Function

Follow these steps to set a polynomial, piecewise-linear, or piecewise-polynomial function for the

pressure jump:

. Check that the Profile Specification of Pressure-Jump option is off in the Fan Dialog Box (p. ).

. Choose polynomial, piecewise-linear, or piecewise-polynomial in the drop-down list to the right of

Pressure-Jump. (If the function type you want is already selected, you can click the Edit... button to

open the dialog box where you will define the function.)

. In the dialog box that appears for the definition of the Pressure Jump function (for example, Fig-

ure . : Polynomial Profile Dialog Box for Pressure Jump Definition (p. )), enter the appropriate values.

These profile input dialog boxes are used the same way as the profile input dialog boxes for temperature-

dependent properties. See Defining Properties Using Temperature-Dependent Functions (p. ) to find

out how to use them.

Figure . : Polynomial Profile Dialog Box for Pressure Jump Definition

. Set any of the optional parameters described below. (optional)

When you define the pressure jump using any of these types of functions, you can choose to limit

the minimum and maximum velocity magnitudes used to calculate the pressure jump. Enabling the

Limit Polynomial Velocity Range option limits the pressure jump when a Min Velocity Magnitude

and a Max Velocity Magnitude are specified.

Important

The values corresponding to the Min Velocity Magnitude and the Max Velocity Mag-

nitude do not limit the flow field velocity to this range. However, this range does limit

the value of the pressure jump, which is a polynomial and a function of velocity, as seen

in Equation . (p. ). If the calculated normal velocity magnitude exceeds the Max

Velocity Magnitude that has been specified, then the pressure jump at the Max Velocity

Magnitude value will be used. Similarly, if the calculated velocity is less than the specified

Min Velocity Magnitude, the pressure jump at the Min Velocity Magnitude will be

substituted for the pressure jump corresponding to the calculated velocity.

You also have the option to use the mass-averaged velocity normal to the fan to determine a single

pressure-jump value for all faces in the fan zone. Turning on Calculate Pressure-Jump from Average

Conditions enables this option.

...... Constant Value

To define a constant pressure jump, follow these steps:

. Turn off the Profile Specification of Pressure-Jump option in the Fan Dialog Box (p. ).

. Choose constant in the drop-down list to the right of Pressure-Jump.

. Enter the value for

in the Pressure-Jump field.

You can follow the procedure below, if it is more convenient:

. Turn on the Profile Specification of Pressure-Jump option.

. Select constant in the drop-down list below Pressure Jump Profile, and enter the value for

in the

Pressure Jump Profile field.

...... User-Defined Function or Profile

For a user-defined pressure-jump function or a function defined in a boundary profile file, you will

follow these steps:

. Choose the appropriate function in the drop-down list below Pressure Jump Profile.

See the Fluent Customization Manual for information about user-defined functions, and Profiles (p. )

for details about profile files.

...... Example: Determining the Pressure Jump Function

This example shows you how to determine the function for the pressure jump. Consider the simple

two-dimensional duct flow illustrated in Figure . : A Fan Located In a 2D Duct (p. ). Air at constant

density enters the . m  . m duct with a velocity of  m/s. Centered in the duct is a fan.

Figure . : A Fan Located In a 2D Duct

Assume that the fan characteristics are as follows when the fan is operating at  rpm:

(Pa)

(

/s)

.

where

is the flow through the fan and

is the pressure rise across the fan. The fan characteristics

in this example follow a simple linear relationship between pressure rise and flow rate. To convert

this into a relationship between pressure rise and velocity, the cross-sectional area of the fan must

be known. In this example, assuming that the duct is . m deep, this area is . m2, so that the

corresponding velocity values are as follows:

(Pa)

(m/s)

.

.

.

.

.

.

The polynomial form of this relationship is the following equation for a line:

(.)

..... Defining Discrete Phase Boundary Conditions for the Fan

fan. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

..... Defining the Fan Swirl Velocity

If you want to set tangential and radial velocity fields on the fan surface to generate swirl in a 3D

problem, follow these steps:

. Turn on the Swirl-Velocity Specification option in the Fan Dialog Box (p. ).

. Specify the fan’s axis of rotation by defining the axis origin (Fan Origin) and direction vector (Fan Axis).

. Set the value for the radius of the fan’s hub (Fan Hub Radius).The default is

to avoid division

by zero in the polynomial.

. Set the tangential and radial velocity functions as polynomial functions of radial distance, constant

values, or user-defined functions.

Important

Important

...... Polynomial Function

To define a polynomial function for tangential or radial velocity, follow the steps below:

. Check that the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity

option is off in the Fan Dialog Box (p. ).

. Enter the coefficients

in Equation . (p. ) or

in Equation . (p. ) in the Tangential- or

Radial-Velocity Polynomial Coefficients field. Enter

first, then

, and so on. Separate each coef-

ficient by a blank space. Remember that the first coefficient is for .

To define a constant tangential or radial velocity, the steps are as follows:

. Turn on the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity

option in the Fan Dialog Box (p. ).

. Select constant in the drop-down list under Tangential or Radial Velocity Profile.

or

in the Tangential or Radial Velocity Profile field.

. Turn off the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity

or

in the Tangential- or Radial-Velocity Polynomial Coefficients field.

For a user-defined tangential or radial velocity function or a function contained in a profile file, follow

the procedure below:

. Turn on the Profile Specification of Tangential or Radial Velocity option.

. Choose the appropriate function from the drop-down list under Tangential or Radial Velocity Profile.

.... Postprocessing for Fans

..... Reporting the Pressure Rise Through the Fan

You can use the Surface Integrals Dialog Box (p. ) to report the pressure rise through the fan, as

described in Surface Integration (p. ). There are two steps to this procedure:

. Create a surface on each side of the fan zone. Use the Transform Surface Dialog Box (p. ) (as described

in Transforming Surfaces (p. )) to translate the fan zone slightly upstream and slightly downstream

to create two new surfaces.

. In the Surface Integrals dialog box, report the average Static Pressure just upstream and just down-

stream of the fan.You can then calculate the pressure rise through the fan.

..... Graphical Plots

Graphical reports of interest with fans are as follows:

Contours or profiles of Static Pressure and Static Temperature.

XY plots of Static Pressure and Static Temperature vs position.

Displaying Graphics (p. ) explains how to generate graphical displays of data.

Important

When generating these plots, be sure to turn off the display of node values so that you

can see the different values on each side of the fan. (If you display node values, the cell

values on either side of the fan will be averaged to obtain a node value, and you will not

see, for example, the pressure jump across the fan.)

A lumped-parameter model for a heat exchange element (for example, a radiator or condenser), is

available in ANSYS Fluent. The radiator boundary type allows you to specify both the pressure drop

and heat transfer coefficient  as functions of the velocity normal to the radiator.

A more detailed heat exchanger model is also available in ANSYS Fluent. See Modeling Heat Ex-

changers (p. ) for details.

.... Radiator Equations

..... Modeling the Pressure Loss Through a Radiator

A radiator is considered to be infinitely thin, and the pressure drop through the radiator is assumed

the radiator,

(.)

is the non-dimensional loss coefficient, which can be specified

as a constant or as a polynomial, piecewise-linear, or piecewise-polynomial function.

(.)

where

are polynomial coefficients and  is the magnitude of the local fluid velocity normal to

the radiator.

..... Modeling the Heat Transfer Through a Radiator

The heat flux from the radiator to the surrounding fluid is given as

(.)

where  is the heat flux,

is the temperature downstream of the heat exchanger (radiator), and

is the radiator temperature. The convective heat transfer coefficient,

, can be specified as a

constant or as a polynomial, piecewise-linear, or piecewise-polynomial function.

For a polynomial, the relationship is of the form

(.)

where

the radiator in m/s.

To define the actual heat flux

, specify a Temperature of absolute zero ( K,  °R, –. °C,

–. °F), and set the constant Heat Flux value.

To define the radiator temperature, enter the value for

in the Temperature field. To define the

Heat-Transfer-Coefficient

, you can specify a polynomial, piecewise-linear, or piecewise-polyno-

mial function of velocity, or a constant value.

(either the entered value or the value calculated using Equation . (p. )) is integrated over

the radiator surface area.

Fluent does not allow you to specify a value less than absolute zero for the radiator temperature.

...... Calculating the Heat Transfer Coefficient

To model the thermal behavior of the radiator, you must supply an expression for the heat transfer

coefficient,

, as a function of the fluid velocity through the radiator,

. To obtain this expression,

consider the heat balance equation:

(.)

where

= heat flux (W/

)

= fluid mass flow rate (kg/s)

= specific heat capacity of fluid (J/kg-K)

= empirical heat transfer coefficient (W/

K)

= external temperature (reference temperature for the liquid) (K)

= temperature downstream from the heat exchanger (K)

= heat exchanger frontal area (

)

Equation . (p. ) can be rewritten as

(.)

where

is the upstream air temperature. The heat transfer coefficient,

, can therefore be com-

puted as

(.)

or, in terms of the fluid velocity,

(.)

)

(.)

where

puted as

(.)

(.)

.... User Inputs for Radiators

Once the radiator zone has been identified (in the Boundary Conditions task page), you will set all

modeling inputs for the radiator in the Radiator Dialog Box (p. ) (Figure . : The Radiator Dialog

Box (p. )), which is opened from the Boundary Conditions Task Page (p. ) (as described in Setting

Cell Zone and Boundary Conditions (p. )).

Figure . : The Radiator Dialog Box

The inputs for a radiator are as follows:

. Identify the radiator zone.

. Define the pressure loss coefficient.

. Define either the heat flux or the heat transfer coefficient and radiator temperature.

If defining the heat flux, specify the Temperature as absolute zero.

. Define the discrete phase boundary condition for the radiator (for discrete phase calculations).

..... Identifying the Radiator Zone

Since the radiator is considered to be infinitely thin, it must be modeled as the interface between

cells, rather than a cell zone. Therefore the radiator zone is a type of internal face zone (where the

faces are line segments in 2D or triangles/quadrilaterals in 3D). If, when you read your mesh into

ANSYS Fluent, the radiator zone is identified as an interior zone, right-click the zone in the tree and

use the Type sub-menu to change it to a radiator zone (for more details, see Changing Cell and

Boundary Zone Types (p. )).

Once the interior zone has been changed to a radiator zone, you can open the Radiator dialog box

and specify the loss coefficient and heat flux information.

..... Defining the Pressure Loss Coefficient Function

To define the pressure loss coefficient

you can specify a polynomial, piecewise-linear, or piecewise-

polynomial function of velocity, or a constant value.

pressure loss coefficient:

Loss Coefficient. (If the function type you want is already selected, you can click the Edit... button to

. In the dialog box that appears for the definition of the Loss Coefficient function (for example, Fig-

ure . : Polynomial Profile Dialog Box for Loss Coefficient Definition (p. )), enter the appropriate

values.These profile input dialog boxes are used the same way as the profile input dialog boxes for

temperature-dependent properties. See Defining Properties Using Temperature-Dependent Func-

tions (p. ) to find out how to use them.

Figure . : Polynomial Profile Dialog Box for Loss Coefficient Definition

To define a constant loss coefficient, follow these steps:

. Choose constant in the Loss Coefficient drop-down list.

in the Loss Coefficient field.

...... Example: Calculating the Loss Coefficient

This example shows you how to determine the loss coefficient function. Consider the simple two-

dimensional duct flow of air through a water-cooled radiator, shown in Figure . : A Simple Duct

with a Radiator (p. ).

Figure . : A Simple Duct with a Radiator

The radiator characteristics must be known empirically. For this case, assume that the radiator to be

modeled yields the test data shown in Table . : Air-side Radiator Data (p. ), which was taken with

a waterside flow rate of  kg/min and an inlet water temperature of . K. To compute the loss

coefficient, it is helpful to construct a table with values of the dynamic head,

, as a function of

pressure drop,

, and the ratio of these two values,

(from Equation . (p. )). (The air

density, defined in Figure . : A Simple Duct with a Radiator (p. ), is . kg/

.) The reduced data

are shown in Table . : Reduced Radiator Data (p. ).

Table . : Air-side Radiator Data

Pressure Drop

Downstream Temp (K)

Upstream Temp (K)

.

.

.

.

.

.

.

.

.

.

.

.

Table . : Reduced Radiator Data

(Pa)

(Pa)

v (m/s)

.

.

.

.

.

.

.

.

.

.

.

.

The loss coefficient is a linear function of the velocity, decreasing as the velocity increases. The form

of this relationship is

(.)

where  is now the absolute value of the velocity through the radiator.

..... Defining the Heat Flux Parameters

As mentioned in Radiator Equations (p. ), you can either define the actual heat flux

in the

Heat Flux field, or set the heat transfer coefficient and radiator temperature

. All inputs are

in the Radiator Dialog Box (p. ).

To define the actual heat flux, specify a Temperature of  K, and set the constant Heat Flux value.

Heat-Transfer-Coefficient, you can specify a polynomial, piecewise-linear, or piecewise-polynomial

function of velocity, or a constant value.

heat transfer coefficient:

Heat-Transfer-Coefficient. (If the function type you want is already selected, you can click the Edit...

button to open the dialog box where you will define the function.)

. In the dialog box that appears for the definition of the Heat-Transfer-Coefficient function, enter the

appropriate values.These profile input dialog boxes are used the same way as the profile input dialog

boxes for temperature-dependent properties. See Defining Properties Using Temperature-Dependent

Functions (p. ) to find out how to use them.

To define a constant heat transfer coefficient, follow these steps:

. Choose constant in the Heat-Transfer-Coefficient drop-down list.

. Enter the value for  in the Heat-Transfer-Coefficient field.

...... Example: Determining the Heat Transfer Coefficient Function

This example shows you how to determine the function for the heat transfer coefficient. Consider

the simple two-dimensional duct flow of air through a water-cooled radiator, shown in Figure . : A

Simple Duct with a Radiator (p. ).

The data supplied in Table . : Air-side Radiator Data (p. ) along with values for the air density

(. kg/

) and specific heat ( J/kg-K) can be used to obtain the following values for the heat

transfer coefficient  :

(W/

K)

.

.

.

.

.

.

The heat transfer coefficient obeys a second-order polynomial relationship (fit to the points in the

table above) with the velocity, which is of the form

(.)

Note that the velocity  is assumed to be the absolute value of the velocity passing through the

radiator.

..... Defining Discrete Phase Boundary Conditions for the Radiator

radiator. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

.... Postprocessing for Radiators

..... Reporting the Radiator Pressure Drop

You can use the Surface Integrals Dialog Box (p. ) to report the pressure drop across the radiator,

as described in Surface Integration (p. ). There are two steps to this procedure:

. Create a surface on each side of the radiator zone. Use the Transform Surface Dialog Box (p. ) (as

described in Transforming Surfaces (p. )) to translate the radiator zone slightly upstream and slightly

downstream to create two new surfaces.

stream of the radiator.You can then calculate the pressure drop across the radiator.

To check this value against the expected value based on Equation . (p. ), you can use the

Surface Integrals dialog box to report the average normal velocity through the radiator. (If the ra-

diator is not aligned with the ,

, or  axis, you will need to use the Custom Field Function Calcu-

lator Dialog Box (p. ) to generate a function for the velocity normal to the radiator.) Once you

have the average normal velocity, you can use Equation . (p. ) to determine the loss coefficient

and then Equation . (p. ) to calculate the expected pressure loss.

..... Reporting Heat Transfer in the Radiator

To determine the temperature rise across the radiator, follow the procedure outlined above for the

pressure drop to generate surfaces upstream and downstream of the radiator. Then use the Surface

Integrals Dialog Box (p. ) (as for the pressure drop report) to report the average Static Temperature

on each surface. You can then calculate the temperature rise across the radiator.

Graphical reports of interest with radiators are as follows:

Important

can see the different values on each side of the radiator. (If you display node values, the

cell values on either side of the radiator will be averaged to obtain a node value, and you

will not see, for example, the pressure loss across the radiator.)

Porous jump conditions are used to model a thin “membrane” that has known velocity (pressure-drop)

characteristics. It is essentially a 1D simplification of the porous media model available for cell zones.

Examples of uses for the porous jump condition include modeling pressure drops through screens

and filters, and modeling radiators when you are not concerned with heat transfer. This simpler model

should be used whenever possible (instead of the full porous media model) because it is more robust

and yields better convergence.

The thin porous medium has a finite thickness over which the pressure change is defined as a combin-

ation of Darcy’s Law and an additional inertial loss term:

(.)

where  is the laminar fluid viscosity,

is the permeability of the medium,

is the pressure-jump

is the velocity normal to the porous face, and

is the thickness of the medium. Appro-

priate values for  and

can be calculated using the techniques described in User Inputs for Porous

Media (p. ).

In a coupled analysis involving Fluent and System Coupling, data can be transferred to and from the

porous jump boundary. For more about System Coupling, see Performing System Coupling Simulations

Using Fluent (p. ). For more information about the data transferred, see Force transferred to System

Coupling from a Porous Jump Boundary (p. ).

Note

The porous jump boundary condition considers only the momentum resistance. Diffusion pro-

cesses are not considered.

Note

In some cases, the pressure-based coupled solver with porous jump boundary conditions may

suffer from convergence issues that do not respond to changes in the coupled solver settings.

This behavior depends on the specific flow configuration and porous jump boundary condition

values. If convergence instability is observed using the coupled pressure-based solver, it is re-

commended that you change the pressure-velocity coupling to one of the segregated schemes.

.... User Inputs for the Porous Jump Model

Once the porous jump zone has been identified (in the Boundary Conditions task page), you will

set all modeling inputs for the porous jump in the Porous Jump Dialog Box (p. ) (Figure . : The

Porous Jump Dialog Box (p. )), which is opened from the Boundary Conditions Task Page (p. )

Figure . : The Porous Jump Dialog Box

The inputs required for the porous jump model are as follows:

. Identify the porous-jump zone.

. Set the Face Permeability of the medium (  in Equation . (p. )).

. Set the Porous Medium Thickness (

).

. Set the Pressure-Jump Coefficient (

).

Note

The unit for the pressure-jump coefficient (C2) is the inverse of length. Should you

want to define different units, you can do so by opening the Units dialog box and se-

lecting length-inverse from the Quantities list.

. Set the Thermal Contact Resistance.

. Define the discrete phase boundary condition for the porous jump (for discrete phase calculations).

. If you have enabled the solar load model, define the Solar Boundary Conditions for the porous jump.

These settings allow you to define the boundary such that it acts as a semi-transparent surface (with re-

spect to the solar radiation calculation only), and therefore allows a portion of the solar radiation to pass

through it. See Solar Ray Tracing (p. ) for details.

..... Identifying the Porous Jump Zone

Since the porous jump model is a 1D simplification of the porous media model, the porous-jump

zone must be modeled as the interface between cells, rather than a cell zone. Therefore the porous-

jump zone is a type of internal face zone (where the faces are line segments in 2D or triangles/quad-

rilaterals in 3D). If the porous-jump zone is not identified as such by default when you read in the

mesh (that is, if it is identified as another type of internal face zone), you can right-click the zone in

the tree and use the Type sub-menu to change it to a porous-jump zone (for more details, see

Changing Cell and Boundary Zone Types (p. )).

After the zone has been changed to a porous jump, you can open the Porous Jump Dialog Box (p. )

(as described in Setting Cell Zone and Boundary Conditions (p. )) and specify the porous jump

parameters listed above.

..... Defining Discrete Phase Boundary Conditions for the Porous Jump

porous jump. See Setting Boundary Conditions for the Discrete Phase (p. ) for details.

.... Postprocessing for the Porous Jump

Postprocessing suggestions for a problem that includes a porous jump are the same as for porous

media problems. See Postprocessing for Porous Media (p. ).

You can edit multiple related boundaries (zones of the same type) at the same time to simplify the

setup process for ANSYS Fluent cases.

Using the Multi Edit dialog box, you can edit or apply selected settings only, to a set of boundaries

without opening multiple different dialog boxes. The dialog box includes colored icons to indicate

which setting(s) will be applied on the selected zones.

To access the Multi Edit dialog box:

. Select the boundaries that you want to edit in the Outline View tree. You can select multiple-boundaries by

holding Ctrl while you left-click.

Alternatively, you can select the boundaries that you want to edit in the Adjacent Face Zones list

of the Adjacency Dialog Box (p. ).

Note

One-sided (or external) walls cannot be selected together with coupled (or internal) walls

for multi-editing.

. Right-click the highlighted boundaries and click Multi Edit....

While Figure . : The Multi Edit Velocity Inlet Dialog Box (p. ) is only for performing a multi-edit

of velocity inlets, the multi-edit functionality is available for the following boundary types:

exhaust fans

inlet vents

intake fans

mass flow inlets

mass flow outlets

outflows

outlet vents

pressure far fields

pressure inlets

pressure outlets

velocity inlets

walls

The setup for the mult-edit versions of these dialog boxes is the same as their non-multi-edit

outflows

walls

counterparts. The multi-edit functionality described in this section is consistent for all of the types.

Editing Multiple Boundary Conditions at Once

Figure . : The Multi Edit Velocity Inlet Dialog Box

The colored icons within the Multi Edit dialog box indicate the states of the various fields:

indicates that the value of this setting varies between the selected boundaries.

indicates that the displayed value will be applied to the selected boundaries when you click Apply.

You can click an icon to change its state, which would be useful if you modify multiple settings, then

realize you made a mistake on one of them. To rectify the mistake, you can simply click

to remove

it, indicating that the setting will not be applied when you click Apply.

Note

For any value entry or selection that results in changes to other fields, do not rely on just

reverting the "master field" (by clicking the

icon) to revert the other affected fields.

If a field has a green check mark (

) next to it, assume that the shown value will be

applied on Apply, regardless of if you revert the initial change that led to the other field

changes.

. The Zone List shows the selected boundaries where the fields denoted with the

icon will be applied.

You can change which boundaries are highlighted in the Zone List, allowing you to selectively apply

settings to a subset of the boundaries in the list. The settings are applied to the selected (highlighted)

zones when you click Apply.

Note

The "master zone" (shown in the Master Zone Name field) cannot be deselected in the

Zone List.

Note

Zone List.

The standard boundary conditions, when imposed on the boundaries of an artificially truncated domain,

result in the reflection of the outgoing pressure waves. As a consequence, the interior domain will

contain spurious wave reflections. Many applications require precise control of the wave reflections

from the domain boundaries to obtain accurate flow solutions. ANSYS Fluent offers several boundary

wave models that can be used to at the domain boundaries to control these spurious wave reflections.

The following boundary acoustic wave models are available:

turbo-specific non-reflecting boundary condition (NRBC) (density-based solver only)

general NRBC (pressure-based and density-based solvers)

impedance boundary condition (pressure-based solver only)

transparent flow forcing (pressure-based solver only)

In the density-based solver, the NRBC models are available for flows using the compressible ideal-gas

law.

In the pressure-based solver, the general NRBC, impedance, and transient flow forcing models available

for transient simulations of compressible flows (including the ideal-gas law, real gas law, species transport,

and compressible mixture models).

Information about the available boundary acoustic wave models is provided in the following sections.

...Turbo-Specific Non-Reflecting Boundary Conditions

... General Non-Reflecting Boundary Conditions

... Impedance Boundary Conditions

...Transparent Flow Forcing Boundary Conditions

Information about turbo-specific NRBCs is provided in the following sections.

.... Overview

....Theory

.... Using Turbo-Specific Non-Reflecting Boundary Conditions

The standard pressure boundary conditions for compressible flow fix specific flow variables at the

boundary (for example, static pressure at an outlet boundary). As a result, pressure waves incident

on the boundary will reflect in an unphysical manner, leading to local errors. The effects are more

pronounced for internal flow problems where boundaries are usually close to geometry inside the

domain, such as compressor or turbine blade rows.

The turbo-specific non-reflecting boundary conditions permit waves to “pass” through the boundaries

without spurious reflections. The method used in ANSYS Fluent is based on the Fourier transformation

of solution variables at the non-reflecting boundary  [] (p. ). Similar implementations have been

investigated by other authors [] (p. ) [] (p. ). The solution is rearranged as a sum of terms

corresponding to different frequencies, and their contributions are calculated independently. While

Boundary Acoustic Wave Models

the method was originally designed for axial turbomachinery, it has been extended for use with radial

turbomachinery.

Note the following limitations of turbo-specific NRBCs:

They are available only with the density-based solver (explicit or implicit).

The current implementation applies to steady compressible flows, with the density calculated using the

ideal gas law.

Inlet and outlet boundary conditions must be pressure inlets and outlets only.

Important

Note that the pressure inlet boundaries must be set to the cylindrical coordinate flow

specification method when turbo-specific NRBCs are used.

Quad-mapped (structured) surface meshes must be used for inflow and outflow boundaries in a 3D geo-

metry (that is, triangular or quad-paved surface meshes are not allowed). See Figure . : Mesh and Pre-

scribed Boundary Conditions in a 3D Axial Flow Problem (p. ) and Figure . : Mesh and Prescribed

Boundary Conditions in a 3D Radial Flow Problem (p. ) for examples.

Important

Note that you may use unstructured meshes in 2D geometries (Figure . : Mesh and

Prescribed Boundary Conditions in a 2D Case (p. )), and an unstructured mesh may

be used away from the inlet and outlet boundaries in 3D geometries.

The turbo-specific NRBC  [] (p. ) has been extended for use on 3D geometries  [] (p. ) by decoup-

ling the tangential flow variations from the radial variations.This approximation works best for geometries

with a blade pitch that is small compared to the radius of the geometry.

Reverse flow on the inflow and outflow boundaries are not allowed. If strong reverse flow is present, then

you should consider using the General NRBCs instead.

NRBCs are not compatible with species transport models.They are mainly used to solve ideal-gas single-

species flow.

Figure . : Mesh and Prescribed Boundary Conditions in a 3D Axial Flow Problem

Figure . : Mesh and Prescribed Boundary Conditions in a 3D Radial Flow Problem

Figure . : Mesh and Prescribed Boundary Conditions in a 2D Case

Turbo-specific NRBCs are based on Fourier decomposition of solutions to the linearized Euler equations.

The solution at the inlet and outlet boundaries is circumferentially decomposed into Fourier modes,

with the 0th mode representing the average boundary value (which is to be imposed as a user input),

and higher harmonics that are modified to eliminate reflections  [] (p. ).

..... Equations in Characteristic Variable Form

In order to treat individual waves, the linearized Euler equations are transformed to characteristic

variable (

) form. If we first consider the 1D form of the linearized Euler equations, it can be shown

that the characteristic variables

are related to the solution variables as follows:

(.)

where

(.)

where  is the average acoustic speed along a boundary zone,

,

,

,

, and  represent perturb-

ations from a uniform condition (for example,

, and so on).

Note that the analysis is performed using the cylindrical coordinate system. All overlined (averaged)

flow field variables (for example,

,

) are intended to be averaged along the pitchwise direction.

In quasi-3D approaches [] (p. ) [] (p. ) [] (p. ), a procedure is developed to determine

the changes in the characteristic variables, denoted by

, at the boundaries such that waves will

not reflect. These changes in characteristic variables are determined as follows:

(.)

where

(.)

(.)

where

(.)

The changes to the outgoing characteristics — one characteristic for subsonic inflow (

), and four

characteristics for subsonic outflow (

,

,

,

) — are determined from extrapolation of the

flow field variables using Equation . (p. ).

The changes in the incoming characteristics — four characteristics for subsonic inflow (

,

,

,

), and one characteristic for subsonic outflow (

) — are split into two components: average

change along the boundary (

), and local changes in the characteristic variable due to harmonic

variation along the boundary (

). The incoming characteristics are therefore given by

(.)

(.)

where

on the inlet boundary or

on the outlet boundary, and

is the grid

index in the pitchwise direction including the periodic point once. The under-relaxation factor  has

a default value of

. Note that this method assumes a periodic solution in the pitchwise direction.

The flow is decomposed into mean and circumferential components using Fourier decomposition.

The 0th Fourier mode corresponds to the average circumferential solution, and is treated according

to the standard 1D characteristic theory. The remaining parts of the solution are described by a sum

of harmonics, and treated as 2D non-reflecting boundary conditions  [] (p. ).

..... Inlet Boundary

For subsonic inflow, there is one outgoing characteristic (

) determined from Equation . (p. ),

and four incoming characteristics (

,

,

,

) calculated using Equation . (p. ). The

,

,

,

average changes in the incoming characteristics are computed from the requirement that the entropy

( ), radial and tangential flow angles (

and

), and stagnation enthalpy (

) are specified. Note

that in ANSYS Fluent you can specify

and

at the inlet, from which

and

are easily obtained.

This is equivalent to forcing the following four residuals to be zero:

(.)

(.)

(.)

(.)

where

(.)

(.)

The average characteristic is then obtained from residual linearization as follows (see also Fig-

ure . : Prescribed Inlet Angles (p. )

(.)

where

(.)

(.)

(.)

and

(.)

(.)

(.)

Figure . : Prescribed Inlet Angles

where

(.)

(.)

(.)

(.)

(.)

(.)

To address the local characteristic changes at each  grid point along the inflow boundary, the fol-

lowing relations are developed  [] (p. ) [] (p. ):

(.)

Note that the relation for the first and fourth local characteristics force the local entropy and stagna-

tion enthalpy to match their average steady-state values.

The characteristic variable

is computed from the inverse discrete Fourier transform of the second

characteristic. The discrete Fourier transform of the second characteristic in turn is related to the

discrete Fourier transform of the fifth characteristic. Hence, the characteristic variable

is computed

along the pitch as follows:

(.)

The Fourier coefficients

are related to a set of equidistant distributed characteristic variables

by the following  [] (p. ):

(.)

where

(.)

and

(.)

The set of equidistributed characteristic variables

(.)

where

(.)

and

(.)

is computed from arbitrary distributed

by

using a cubic spline for interpolation, where

(.)

For supersonic inflow the user-prescribed static pressure (

) along with total pressure (

) and

total temperature (

) are sufficient for determining the flow condition at the inlet.

..... Outlet Boundary

For subsonic outflow, there are four outgoing characteristics (

,

,

, and

) calculated using

Equation . (p. ), and one incoming characteristic (

) determined from Equation . (p. ).

The average change in the incoming fifth characteristic is given by

(.)

where  is the current averaged pressure at the exit plane and

is the desirable average exit

pressure (this value is specified by you for single-blade calculations or obtained from the assigned

profile for mixing-plane calculations). The local changes (

) are given by

(.)

is computed along the pitch as follows:

(.)

are related to two sets of equidistantly distributed characteristic variables

(

and

, respectively) and given by the following  [] (p. ):

(.)

where

(.)

(.)

The two sets of equidistributed characteristic variables (

and

) are computed from arbitrarily

distributed

and

characteristics by using a cubic spline for interpolation, where

(.)

(.)

For supersonic outflow all flow field variables are extrapolated from the interior.

..... Updated Flow Variables

Once the changes in the characteristics are determined on the inflow or outflow boundaries, the

changes in the flow variables

can be obtained from Equation . (p. ). Therefore, the values

of the flow variables at the boundary faces are as follows:

(.)

(.)

(.)

(.)

(.)

Important

If you intend to use turbo-specific NRBCs in conjunction with the density-based implicit

solver, it is recommended that you first converge the solution before turning on turbo-

specific NRBCs, then converge it again with turbo-specific NRBCs turned on. If the solution

is diverging, then you should lower the CFL number. These steps are necessary because

only approximate flux Jacobians are used for the pressure-inlet and pressure-outlet

boundaries when turbo-specific NRBCs are activated with the density-based implicit solver.

The procedure for using the turbo-specific NRBCs is as follows:

. Turn on the turbo-specific NRBCs using the non-reflecting-bc text command:

define → boundary-conditions → non-reflecting-bc → turbo-specific-nrbc

→ enable?

If you are not sure whether or not NRBCs are turned on, use the show-status text command.

. Perform NRBC initialization using the initialize text command:

→ initialize

If the initialization is successful, a summary printout of the domain extent will be displayed. If the

initialization is not successful, an error message will be displayed indicating the source of the

problem. The initialization will set up the pressure-inlet and pressure-outlet boundaries for use

with turbo-specific NRBCs.

Important

Important

. If necessary, modify the parameters in the set/ submenu:

→ set

under-relaxation

allows you to set the value of the under-relaxation factor  in Equation . (p. ).The default

value is

.

allows you to set the discretization scheme.The default is to use higher-order reconstruction if

verbosity

allows you to control the amount of information printed to the console during an NRBC calculation.

: silent

: basic information (default)

: detailed information (for debugging purposes only)

..... Using the NRBCs with the Mixing-Plane Model

If you want to use the NRBCs with the mixing-plane model you must define the mixing plane interfaces

as pressure-outlet and pressure-inlet zone type pairs.

Important

Turbo-specific NRBCs should not be used with the mixing-plane model if reverse flow is

present across the mixing-plane.

..... Using the NRBCs in Parallel ANSYS Fluent

When the turbo-specific NRBCs are used in conjunction with the parallel solver, all cells in each

boundary zone, where NRBCs will be applied, must be located or contained within a single partition.

You can ensure this by manually partitioning the mesh (see Partitioning the Mesh Manually and

Balancing the Load (p. ) for more information).

Information about general NRBCs is provided in the following sections.

.... Restrictions and Limitations

.... Using the General Non-Reflecting Boundary Condition

The general non-reflecting boundary conditions in ANSYS Fluent are based on characteristic wave

relations derived from the Euler equations. In the density-based solver, the non-reflecting boundary

conditions are applied only on pressure-outlet boundary conditions. In the pressure-based solver they

are applied on pressure-inlet, pressure-outlet, velocity-inlet and mass-flux boundary conditions. To

obtain the primitive flow quantities (

), reformulated Euler equations are solved on the

boundary of the domain in an algorithm similar to the flow equations applied to the interior of the

domain.

Unlike the turbo-specific NRBC, the general NRBC method is not restricted by geometric constraints

or mesh type. However, good cell skewness near the boundaries where the NRBCs can be applied

for better convergence.

Note the following restrictions and limitations on the general NRBCs:

The general NRBC is not available if the target mass flow rate is activated in the pressure-outlet dialog

box.

The general NRBC using the density-based solver is available only with compressible flow while using the

ideal-gas law.

Important

The general NRBC using the density-based solver should not be used with the wet steam

or real gas models.

The general NRBCs using the density-based solver are not compatible with species transport and mixture

fraction transport models (for premixed and partially-premixed models).They are mainly used to solve

ideal-gas single-component flow.

The general NRBCs using the pressure-based solver are not compatible with steady-state cases or

the Eulerian multiphase model. For VOF or mixture multiphase cases that involve compressible

gases or compressible liquids, only pressure inlets and pressure outlets can enable the non-reflecting

boundary condition option. Note that some small reflections may still occur from NRBC boundaries

when secondary-phase volume fractions are nonzero at the boundaries.

General NRBCs are derived by first recasting the Euler equations in an orthogonal coordinate system

(

) such that one of the coordinates,

, is normal to the boundary Figure . : The Local Ortho-

gonal Coordinate System onto which Euler Equations are Recasted for the General NRBC Method (p. ).

The characteristic analysis  [] (p. ) [] (p. ) is then used to modify terms corresponding to

waves propagating in the

normal direction. When doing so, a system of equations can be written

to describe the wave propagation as follows:

(.)

Where

,

and

and

,

and

are the velocity components in the coordinate

system (

,

,

). The equations above are solved on non-reflecting boundaries, along with the interior

governing flow equations, using similar time stepping algorithms to obtain the values of the primitive

flow variables (

).

Important

Note that a transformation between the local orthogonal coordinate system (

,

,

) and

the global Cartesian system (X, Y, Z) must be defined on each face on the boundary to

obtain the velocity components ( ,

,

) in a global Cartesian system.

,

Figure . : The Local Orthogonal Coordinate System onto which Euler Equations are Recasted

for the General NRBC Method

The

terms in the transformed Euler equations contain the outgoing and incoming characteristic

wave amplitudes,

, and are defined as follows:

(.)

From characteristic analyses, the wave amplitudes,

, are given by:

(.)

The outgoing and incoming characteristic waves are associated with the characteristic velocities of

the system (i.e eigenvalues),

, as seen in Figure . : Waves Leaving and Entering a Boundary Face

on Inflow and Outflow Boundaries. The Wave Amplitudes are Shown with the Associated Eigenvalues

for a Subsonic Flow Condition (p. ). These eigenvalues are given by:

(.)

Figure . : Waves Leaving and Entering a Boundary Face on Inflow and Outflow Boundaries.

The Wave Amplitudes are Shown with the Associated Eigenvalues for a Subsonic Flow Condition

For subsonic flow leaving a boundary, four waves leave the domain (associated with positive eigen-

values

,

,

, and

) and one enters the domain (associated with negative eigenvalue

). For

subsonic flow entering a boundary, four waves enter the domain (associated with the negative eigen-

values

,

,

,

) and one leaves the domain (associated with a positive eigenvalue

).

To solve Equation . (p. ) on a boundary, the amplitude of the incoming and outgoing waves

must be first determined. The amplitude of outgoing waves are computed from Equation . (p. )

by using extrapolated values of flow derivatives

,

,

,

, and

from inside the domain. The

,

,

,

, and

amplitude of the incoming waves are computed as follows. The amplitude of waves

,

, for tangential

velocity components, is set to zero. The amplitude of the incoming pressure and entropy waves are

computed from the Linear Relaxation Method (LRM) of Poinsot [] (p. ) [] (p. ). The LRM

method sets the value of the incoming wave amplitude to be proportional to the differences between

the local primitive variable on a boundary face and the imposed boundary value. The expression for

the amplitudes depends on the boundary type as shown below:

. Pressure Outlet

(.)

where

is the imposed pressure at the exit boundary,

is the relaxation factor, and  is the

local pressure value at the boundary.

In general, the desirable average pressure on a non-reflecting boundary can be either relaxed to-

ward a pressure value at infinity or enforced to be equivalent to some desired pressure at the exit

of the boundary.

In the case of a backflow, the pressure-based solver has two options for specifying pressure at

the boundary; static pressure or total pressure. If the static pressure option is selected, the pressure

at infinity is equal to the pressure defined in the boundary dialog box. If the total pressure option

is selected, the pressure at infinity is a total pressure that is computed from the value in the dialog

box. For the density-based solver, the total pressure option is used and no other options are

If you want the average pressure at the boundary to relax toward  at infinity (that is

),

the suggested

factor is given by:

(.)

),

(.)

where  is the acoustic speed,

is the domain size,

is the maximum Mach number in the

domain, and

is the under-relaxation factor (default value is . ). On the other hand, if the desired

average pressure at the boundary is to approach a specific imposed value at the boundary, then

the

(.)

where the default value for

is .

Important

The desired average pressure option is only available for the density-based solver.

. Pressure Inlet:

(.)

where the imposed pressure,

, and density,

, are computed from the specified total

pressure and total temperature.

. Mass Flux Boundary:

(.)

where the imposed exit velocity and density are computed from specific mass flux and total

temperature.

. Velocity Inlet:

(.)

where the imposed velocity,

, is specified at the boundary and the imposed density is

computed from the specified boundary temperature and extrapolated pressure.

The general Non-Reflecting Boundary Condition is available for use in the Pressure Outlet dialog

box when either the density-based (with ideal gas law) or pressure-based solvers are activated to

solve for compressible flows. The general Non-Reflecting Boundary Condition is available for use in

the Pressure Inlet, Mass-Flow Inlet, and Velocity Inlet dialog boxes when the pressure-based solver

is activated to solve for compressible flows.

The example below shows you how to enable the general Non-Reflecting Boundary Condition in the

Pressure Outlet dialog box. You would follow similar steps for the other boundary condition types

mentioned above.

.

Select pressure-outlet from the Boundary Conditions task page and click the Edit... button.

.

In the Pressure Outlet dialog box, choose Non Reflecting under Acoustic Wave Model.

Figure . : The Pressure Outlet Dialog Box With the Non-Reflecting Boundary Enabled

.

For the density-based solver, select one of the two Exit Pressure Specification options: Pressure at

Infinity or Average Boundary Pressure.The pressure-based solver uses the Pressure at Infinity option

and the Exit Pressure Specification drop-down list is not available.

a.

The Pressure at Infinity boundary is typically used in unsteady calculations or when the exit

pressure value is imposed at infinity.The boundary is designed so that the pressure at the

boundary relaxes toward the imposed pressure at infinity.The speed at which this relaxation takes

place is controlled by the parameter, sigma, which can be adjusted in the TUI:

define → boundary-conditions → non-reflecting-bc → general-nrbc →

set

In the set/ submenu, you can set the sigma value. The default value for sigma is ..

b.

The Average Boundary Pressure specification is usually used in steady-state calculations when

you want to force the average pressure on the boundary to approach the exit pressure value.The

matching of average exit pressure to the imposed average pressure is controlled by the parameter

sigma2 which can be adjusted in the TUI:

set

set

In the set/ submenu, you can set the sigma2 value. The default value for sigma2 is ..

Important

There is no guarantee that the sigma2 value of . will force the average boundary

pressure to match the specified exit pressure in all flow situations. In the case where

the desired average boundary pressure has not been achieved, you can intervene to

adjust the sigma2 value so that the desired average pressure on the boundary is

approached.

.

For the pressure-based solver, you can select one of two Backflow Pressure Specification options:

Static Pressure or Total Pressure. For the density-based solver, the Backflow Pressure Specification

is not shown and the Total Pressure option is used by default. Note that backflow is not allowed for

pressure inlets, mass-flow inlets, or velocity inlets.

Important

For the pressure-based solver, you should choose Direction Vector or From Neigh-

boring Cell as the Backflow Direction Specification Method if the flow is tangential

to the boundary. You should not select the Normal to the Boundary option for

Backflow Direction Specification Method in this case because the face velocity

components for this case will be computed from flux as zero during initialization. This

initialization will cause the solver convergence to fail.

Usually, the solver can operate at higher CFL values without the NRBCs being turned on. Therefore,

the best practice is to first achieve a good stable solution (not necessarily converged) before activating

the non-reflecting boundary condition. In many flow situations, the CFL value must be reduced from

the normal operation to keep the solution stable. This is particularly true with the density-based im-

plicit solver since the boundary update is done in an explicit manner. A typical CFL value in the

density-based implicit solver, with the NRBC activated, is . and . in the pressure-based solver.

The impedance boundary condition (IBC) lies in between a traditional reflective boundary condition

and a fully non-reflective boundary condition. It provides the ability to specify a partial reflection in

the range from full-reflection to no-reflection. Impedance is a complex value; it is the reflection that

changes the amplitude and the phase of the incoming wave. The use of impedance boundary conditions

comes in cases where the flow in the simulation is highly influenced by reflected waves from objects

outside the computational domain. In such cases the acoustic wave interaction from the larger domain

can be modeled in the smaller domain through the use of impedance boundary conditions.

The impedance boundary condition is available only in the pressure-based solver. It is incompatible

with steady-state flow, multiphase, or compressible liquid models (compressible-liquid method for

density).

Impedance specifies an acoustic resistance in the frequency domain. It is a characteristic of the

properties of the media and specific geometry described by a ratio of the pressure perturbation to

the normal velocity perturbation at the boundary Blackstock [[] (p. )].

(.)

(.)

where apostrophe denotes acoustic perturbation and hat denotes quantity in the frequency domain.

Fluent is a time domain solver. It cannot use the impedance from the frequency domain directly. The

above expression and all its variables have to be converted to the time domain. After the conversion

the relation between pressure and normal velocity perturbations is expressed through a convolution

integral.

(.)

If impedance,

, is unbounded in the time domain, then admittance is used (admittance is the

inverse of impedance). Fluent uses the reflection coefficient instead of impedance/admittance, to

uniformly treat unbounded cases Fung [[] (p. )]. The reflection coefficient is a ratio between re-

flected and incoming wave amplitudes at the boundary. It is expressed through the impedance as:

(.)

Using a reflection coefficient, the relation between pressure and normal velocity perturbation is:

(.)

The discretized form of this expression is used in Fluent to connect acoustic pressure and normal

velocity. The computed acoustic perturbations are superimposed onto the pressure and velocity from

non-reflecting boundary condition equations. The non-reflecting boundary condition equations provide

mean flow values at the boundary, which drive the flow in the domain.

The data for the reflection coefficient are available in the frequency domain. As such they usually do

not satisfy the causality and reality conditions. Fluent asks you to provide the reflection coefficient

data in the form of a special approximation. This approximation is based on the system theory, which

ensures that the reflection coefficient in the time domain will satisfy the above conditions Fung

[[] (p. )]. The reflection coefficient is represented as a sum of zero, first and second order systems.

The zero system is described with a real value, the first order system is described with a real pole,

and the second order system is described with a pair of complex conjugate poles. Introducing a system

variable,

the complete approximation for the reflection coefficient is:

(.)

where

is a real term,

is a number of real poles,

and

are real pole and its amplitude,

is

a number of complex conjugate pole pairs,

,

are real and imaginary part of the complex conjugate

pole,

and

are real and imaginary part of the amplitude of the complex pole.

To obey the causality and reality conditions, real pole

, real

and imaginary part

of the complex

conjugate pole should be positive. The passivity condition requires that the absolute value of zero

order term

be less than . The above restrictions are enforced in the user interface. In addition you

should ensure that the absolute value of the reflection coefficient computed by this formula is less

than .

The impedance data can be obtained from measurements or from an acoustic solver. Running these

data through a mathematics package will provide an approximation in terms of first and second order

poles.

.... Using the Impedance Boundary Condition

The example below shows you how to enable the impedance boundary condition (IBC) in the Pressure

Outlet dialog box. Similarly, you can enable IBC in the Pressure Inlet, Velocity Inlet, and Mass-Flow

Inlet dialog boxes for compressible flows with the pressure-based solver.

.

Select pressure-outlet from the Boundary Condition task page and click the Edit... button.

.

In the Pressure Outlet dialog box, choose Impedance under Acoustic Wave Model.

The dialog box will expand to reveal Impedance Parameters.

.

In Impedance Parameters enter data for the reflection coefficient according to the approximation

formula (Equation . (p. )).

a.

Specify the Zero Order Term,

.

b.

Under Real Pole Series, set the Number of Real Poles and for each real pole specify the Pole,

,

and the Amplitude,

.

c.

Under Complex Pole Series, set the Number of Complex Poles and for each complex pole pair,

specify Pole Real,

, Pole Imaginary,

, Amplitude Real,

, and Amplitude Imaginary,

.

Important

If flow is tangential to the boundary, then specify either From Neighboring Cell or

Direction Vector for Back flow Direction Specification Method. Do not select Normal

to the boundary because this computes the face velocity components from flux to

zero values during initialization, which impairs solver convergence.

The IBC is implemented on top of the non-reflective boundary condition.

Note

The mean flow in the domain should be well established before enabling IBC.

The cell acoustic Courant (CFL) number should be less than  in cells adjacent to the

boundary where you define an impedance acoustic boundary condition. (For the definition

of the Cell Acoustic Courant Number, refer to Field Function Definitions (p. )).

With the impedance acoustic boundary condition, you need to tighten the convergence

criteria for continuity to 1e- in order to increase the number of coupling iterations between

the impedance boundary condition calculation and the solver at each time step.

It is often desirable in simulations to cut a domain down to a smaller region to model only a part of

the larger domain. The treatment at the boundaries created when doing so should be consistent with

a slice through the larger domain. That is, incoming transients should be allowed to enter the compu-

tational domain and outgoing transients should leave the domain without reflections. Artificial numer-

ical reflections at the boundaries can significantly affect the predicted flow, particularly if the geometry

of the numerical domain has Eigen-frequencies that match the frequencies of physical waves

propagating through the flow.

The transparent flow forcing treatment provides the capability to model incoming waves while allowing

outgoing waves to pass through the boundaries without reflection. It is available in transient simulations

of compressible flow using the pressure-based solver and can be applied for velocity inlets, mass-flow

inlets, pressure inlets, and pressure outlets.

The transparent flow forcing condition is available only in the pressure-based solver and it is incom-

patible with steady-state flow, multiphase, and compressible liquid models (those using the compress-

ible-liquid method for density).

The transparent flow forcing boundary condition is implemented on top of the non-reflecting

boundary condition. The non-reflecting part of the boundary condition drives the mean flow. The

transient flow at the boundary is split into two waves [] (p. ): incoming wave,

, and

outgoing wave,

. In the acoustic limit, the intensities of the waves are expressed through

pressure and normal velocity perturbations as:

where

is the specific impedance of the mean flow with density,

, and speed of sound, . The

outgoing wave intensity,

, is computed internally while the incoming wave intensity,

, is user-specified through a user-defined profile.

.... Using the Transparent Flow Forcing Boundary Condition

The transparent flow forcing (TFF) boundary condition is available at velocity inlets, mass-flow inlets,

pressure inlets, and pressure outlets when simulating transient compressible flow using the pressure-

based solver. The steps for using the transparent flow forcing boundary condition are as follows:

.

Create a profile for the incoming wave intensity on the boundary.The profile can be created either as

a profile file as described in Profiles (p. ) or using the DEFINE_PROFILE macro as described in

Fluent Customization Manual. In the profile definition, you will specify the wave intensity as a function

of position and time. For the incoming wave, the pressure and normal velocity perturbations satisfy

the relation:

Using this relation the incoming wave intensity at the boundary can be computed from any of

the flow perturbation quantities.

from acoustic pressure,

from acoustic velocity,

from acoustic mass flux,

where  is the speed of sound and

is the acoustic impedance.

.

.

Open the boundary condition settings dialog box for the boundary zone of interest (Setting Cell Zone

.

On the Momentum tab, select Transparent Flow Forcing under Acoustic Wave Model.

.

Under Transparent Flow Forcing Parameters, select your profile from the drop-down list next to In-

coming Wave.

Important

If flow is tangential to the boundary, then specify either From Neighboring Cell or Direction

Vector for Back flow Direction Specification Method. Do not select Normal to the boundary

because this computes the face velocity components from flux to zero values during initializa-

tion, which impairs solver convergence.

The TFF condition is implemented on top of the non-reflective boundary condition. Choose a

time step that will not make the CFL number exceed a value of  in the cells adjacent to the

TFF boundary.

The mean flow in the domain should be well established before enabling TFF.

The user-defined fan model in ANSYS Fluent allows you to periodically regenerate a profile file that can

be used to specify the characteristics of a fan, including pressure jump across the fan, and radial and

swirling components of velocity generated by the fan.

For example, consider the calculation of the pressure jump across the fan. You can, through the

standard interface, input a constant for the pressure jump, specify a polynomial that describes the

pressure jump as a function of axial velocity through the fan, or use a profile file that describes the

User-Defined Fan Model

pressure jump as a function of the axial velocity or location at the fan face. If you use a profile file, the

same profile will be used consistently throughout the course of the solution. Suppose, however, that

you want to change the profile as the flow field develops. This would require a periodic update to the

profile file itself, based upon some instructions that you supply. The user-defined fan model is designed

to help you do this.

To use this model, you need to generate an executable that reads a fan profile file that is written by

ANSYS Fluent, and writes out a modified one, which ANSYS Fluent will then read. The source code for

this executable can be written in any programming language (Fortran or C, for example). Your program

will be called and executed automatically, according to inputs that you supply through the standard

Information about the user-defined fan model is provided in the following sections.

... Steps for Using the User-Defined Fan Model

... Example of a User-Defined Fan

To make use of the user-defined fan model, follow the steps below.

. In your model, identify one or more interior faces to represent one or more fan zones.

Setup →

. Input the name of your executable and the instructions for reading and writing profile files in the User-

Defined Fan Model Dialog Box (p. ).

User Defined → Model Specific → Fan Model...

. Initialize the flow field and the profile files.

. Enter the fan parameters using the standard Fan Dialog Box (p. ) (opened from the Boundary Conditions

Task Page (p. )).

. Perform the calculation.

Usage of the user-defined fan model is best demonstrated by an example. With this in mind, consider

the domain shown in Figure . : The Inlet, Fan, and Pressure Outlet Zones for a Circular Fan Operating

in a Cylindrical Domain (p. ). An inlet supplies air at  m/s to a cylindrical region, . m long and

. m in diameter, surrounded by a symmetry boundary. At the center of the flow domain is a circular

fan. A pressure outlet boundary is at the downstream end.

Figure . : The Inlet, Fan, and Pressure Outlet Zones for a Circular Fan Operating in a Cylindrical

Domain

Solving this problem with the user-defined fan model will cause ANSYS Fluent to periodically write

out a radial profile file with the current solution variables at the fan face. These variables (static pressure,

pressure jump, axial, radial, and swirling (tangential) velocity components) will represent averaged

quantities over annular sections of the fan. The sizes of the annular regions are determined by the size

of the fan and the number of radial points to be used in the profiles.

Once the profile file is written, ANSYS Fluent will invoke an executable, which will perform the following

tasks:

. Read the profile file containing the current flow conditions at the fan.

. Perform a calculation to compute new values for the pressure jump, radial velocity, and swirl velocity for

the fan.

. Write a new profile file that contains the results of these calculations.

ANSYS Fluent will then read the new profile file and continue with the calculation.

the fan.

.... Setting the User-Defined Fan Parameters

Specification of the parameters for the user-defined fan begins in the User-Defined Fan Model Dialog

Box (p. ) (Figure . : The User-Defined Fan Model Dialog Box (p. )).

Figure . : The User-Defined Fan Model Dialog Box

In this dialog box, you can select the fan zone(s) on which your executable will operate under Fan

Zones. In this example, there is only one fan, fan-. If you have multiple fan zones in a simulation,

for which you have different profile specifications, you can select them all at this point. Your executable

will be able to differentiate between the fan zones because the zone ID for each fan is included in

the solution profile file. The executable will be invoked once for each zone, and separate profile files

will be written for each.

The executable file will be called on to update the profile file periodically, based on the input for the

Iteration Update Interval. An input of , as shown in the dialog box, means that the fan executable

in this example will act every  iterations to modify the profile file.

The number of points in the profile file to be written by ANSYS Fluent is entered under Output Profile

Points. This profile file can have the same or a different number of points as the one that is written

by the external executable.

Finally, the name of the executable should be entered under External Command Name. In the current

example, the name of the executable is fan-model.

Important

Important

If the executable is not located in your working directory, then you must type the complete

path to the executable.

.... Sample User-Defined Fan Program

The executable file will be built from the Fortran program, fantest.f, which is shown below.

c

c  This program is invoked at intervals by ANSYS Fluent to

c  read a profile-format file that contains radially

c  averaged data at a fan face, compute new pressure-jump

c  and swirl-velocity components, and write a new profile

c  file that will subsequently be read by ANSYS Fluent to

c  update the fan conditions.

c

c  Usage: fantest input_profile output_profile

c

integer npmax

parameter (npmax = )

integer inp         ! input: number of profile points

integer iptype      ! input: profile type (=radial, =point)

real ir(npmax)      ! input: radial positions

real ip(npmax)      ! input: pressure

real idp(npmax)     ! input: pressure-jump

real iva(npmax)     ! input: axial velocity

real ivr(npmax)     ! input: radial velocity

real ivt(npmax)     ! input: tangential velocity

character* zoneid

integer rfanprof    ! function to read a profile file

integer status

c

status = rfanprof(npmax,zoneid,iptype,

$  inp,ir,ip,idp,iva,ivr,ivt)

if (status.ne.) then

write(*,*) ’error reading input profile file’

else

do  i = , inp

idp(i) = . - . *iva(i)

ivt(i) = . *ir(i)

ivr(i) = .

continue

call wfanprof(,zoneid,iptype,inp,ir,idp,ivr,ivt)

endif

stop

end

After the variable declarations, which have comments on the right, the subroutine rfanprof is

ivr(i) = .

continue

endif

stop

end

called to read the profile file, and pass the current values of the relevant variables (as defined in the

declaration list) to fantest. A loop is done on the number of points in the profile to compute new

values for:

The pressure jump across the fan, idp, which in this example is a function of the axial velocity, iva.

The swirling or tangential velocity, ivt, which in this example is proportional to the radial position, ir.

The radial velocity, ivr, which in this example is set to zero.

After the loop, a new profile is written by the subroutine wfanprof, shown below. (For more inform-

ation on profile file formats, see Profile File Formats (p. ).)

subroutine wfanprof(unit,zoneid,ptype,n,r,dp,vr,vt)

c

c  writes an ANSYS Fluent profile file for input by the

c  user fan model

c

integer unit       ! output unit number

integer ptype      ! profile type (=radial, =point)

integer n          ! number of points

real r(n)          ! radial position

real dp(n)         ! pressure jump

real vr(n)         ! radial velocity

real vt(n)         ! tangential velocity

character* typenam

if (ptype.eq.) then

typenam = ’radial’

else

typenam = ’point’

endif

write(unit,*) ’((’, zoneid(:index(zoneid,’\’)-), ’ ’,

$  typenam, n, ’)’

write(unit,*) ’(r’

write(unit,) r

write(unit,*) ’)’

write(unit,*) ’(pressure-jump’

write(unit,) dp

write(unit,*) ’(radial-velocity’

write(unit,) vr

write(unit,*) ’(tangential-velocity’

write(unit,) vt

format((e15.,1x))

return

end

return

end

This subroutine will write a profile file in either radial or point format, based on your input for the

integer ptype. (See Profiles (p. ) for more details on the types of profile files that are available.)

The names that you use for the various profiles are arbitrary. Once you have initialized the profile

files, the names you use in wfanprof will appear as profile names in the Fan Dialog Box (p. ).

.... Initializing the Flow Field and Profile Files

The next step in the setup of the user-defined fan is to initialize (create) the profile files that will be

used. To do this, first initialize the flow field with the Solution Initialization Task Page (p. ) (using

the velocity inlet conditions, for example), and then type the command (update-user-fans) in

the console window. (The parentheses are part of the command, and must be typed in.)

This will create the profile names that are given in the subroutine wfanprof.

.... Selecting the Profiles

Once the profile names have been established, you will need to visit the Fan Dialog Box (p. ) (Fig-

ure . : The Fan Dialog Box (p. )) to complete the problem setup. (See Fan Boundary Condi-

tions (p. ) for general information on using the Fan dialog box.)

At this time, the Fan Axis, Fan Origin, and Fan Hub Radius can be entered, along with the choice

of profiles for the calculation of pressure jump, tangential velocity, and radial velocity. With the profile

options enabled, you can select the names of the profiles from the drop-down lists. In the dialog box

above, the selected profiles are named fan_8_pressure_jump, fan_8_tangential_velocity, and

fan_8_radial_velocity, corresponding to the names that were used in the subroutine wfanprof.

.... Performing the Calculation

The solution is now ready to run. As it begins to converge, the report in the console window shows

that the profile files are being written and read every  iterations:

iter   continuity   x-velocity   y-velocity   z-velocity          k

! residual normalization factors changed (continuity

.0000e+   .0000e+   .0000e+   .0000e+   .0000e+

.0000e+   .0000e+   .0000e+   .0000e+   .4933e-

.8870e-   .2663e-   .3802e-   .5822e-   .1033e-

. . . . . .

. . . . . .

. . . . . .

.1779e-   .8139e-   .0497e-   .9609e-   .8612e-

Writing "fan--out.prof"...

Done.

Reading "fan--in.prof"...

Reading profile file...

"fan-"  radial-profile points, r, pressure-jump,

radial-velocity, tangential-velocity.

Done.

.7612e-   .4618e-   .5194e-   .4538e-   .4569e-

.6895e-   .3699e-   .0316e-   .0280e-   .1169e-

. . . . . .

. . . . . .

. . . . . .

The file fan--out.prof is written out by ANSYS Fluent and read by the executable fantest. It

contains values for pressure, pressure jump, axial velocity, radial velocity, and tangential velocity at

radial locations at the site of the fan. The file fan--in.prof is generated by fantest and

contains updated values for pressure jump and radial and tangential velocity only. It is therefore a

smaller file than fan--out.prof. The prefix for these files takes its name from the fan zone with

which the profiles are associated. An example of the profile file fan--in.prof is shown below.

This represents the last profile file to be written by fantest during the convergence history.

((fan- radial )

(r

.24295786E- .33130988E- .41966137E- .50801374E- .59636571E-

.68471842E- .77307090E- .86142287E- .94963484E- .95353782E-

)

(pressure-jump

.10182057E+ .98394081E+ .97748657E+ .97787750E+ .97905228E+

.98020668E+ .98138817E+ .98264198E+ .98469681E+ .98478783E+

)

(radial-velocity

.00000000E+ .00000000E+ .00000000E+ .00000000E+ .00000000E+

)

(tangential-velocity

.48591572E+ .66261977E+ .83932275E+ .10160275E+ .11927314E+

.13694369E+ .15461419E+ .17228458E+ .18992697E+ .19070756E+

)

.... Results

A plot of the transverse velocity components at the site of the fan is shown in Figure . : Transverse

Velocities at the Site of the Fan (p. ). As expected, there is no radial component, and the tangential

(swirling) component increases with radius.

Figure . : Transverse Velocities at the Site of the Fan

As a final check on the result, an XY plot of the static pressure as a function of  position is shown

(Figure . : Static Pressure Jump Across the Fan (p. )). This XY plot is made on a line at =. m,

or at about half the radius of the duct. According to the input file shown above, the pressure jump

at the site of the fan should be approximately . Pa/m. Examination of the figure supports this

finding.

Figure . : Static Pressure Jump Across the Fan

finding.

Profiles can be boundary conditions, cell zone conditions, and initial conditions for discrete phases.

ANSYS Fluent provides a very flexible profile definition mechanism. This feature allows you to use ex-

perimental data, data calculated by an external program, or data written from a previous solution using

the Write Profile Dialog Box (p. ) (as described in Reading and Writing Profile Files (p. )) as the

boundary condition for a variable.

Information about profiles is presented in the following subsections:

... Profile Specification Types

... Profile File Formats

... Using Profiles

... Reorienting Profiles

... Replicating Profiles

... Defining Transient Cell Zone and Boundary Conditions

The following is a list of the six types of profiles that can be read into ANSYS Fluent, as well as inform-

ation about the interpolation method employed by ANSYS Fluent for each type.

Point profiles are specified by an unordered set of  points:

for 2D problems or

for

3D problems, where

. Profiles written using the Write Profile dialog box and profiles of experimental

data in random order are examples of point profiles.

ANSYS Fluent will interpolate the point cloud to obtain values at the boundary faces. The default

interpolation method for the unstructured point data is zeroth order. That is, for each cell face at

the boundary, the solver uses the value from the profile file located closest to the cell. Therefore,

to get an accurate specification of an inlet profile using the default interpolation method, your

Profiles

profile file should contain a sufficiently high point density. For information about other available

Profiles

interpolation methods for point profiles, see Using Profiles (p. ).

Line profiles are specified for 2D problems by an ordered set of  points:

, where

. Zeroth-

order interpolation is performed between the points. An example of a line profile is a profile of data obtained

from an external program that calculates a boundary-layer profile.

Mesh profiles are specified for 3D problems by an

by  mesh of points:

, where

and

. Zeroth-order interpolation is performed between the points. Examples of mesh profiles are

profiles of data from a structured mesh solution and experimental data in a regular array.

Radial profiles are specified for 2D and 3D problems by an ordered set of  points:

, where

.

The data in a radial profile are a function of radius only. Linear interpolation is performed between the

points, which must be sorted in ascending order of the  field.The axis for the cylindrical coordinate system

is determined as follows:

– For 2D problems, it is the -direction vector through (,).

– For 2D axisymmetric problems, it is the -direction vector through (,).

– For 3D problems involving a swirling fan, it is the fan axis defined in the Fan Dialog Box (p. ) (unless

you are using local cylindrical coordinates at the boundary, as described below).

– For 3D problems without a swirling fan, it is the rotation axis of the adjacent fluid zone, as defined in the

Fluid Dialog Box (p. ) (unless you are using local cylindrical coordinates at the boundary, as described

below).

– For 3D problems in which you are using local cylindrical coordinates to specify conditions at the

boundary, it is the axis of the specified local coordinate system.

below).

Axial profiles are specified for 3D problems by an ordered set of  points:

, where

.The data

in an axial profile are a function of the axial direction. Linear interpolation is performed between the points,

which must be sorted in ascending order of the  field.

Transient profiles are specified for 2D and 3D profiles by an ordered set of  points:

.

Linear interpolations are done between the points which must be sorted in ascending order of the  (time

or crank angle) field. Examples of transient profiles are transient cell zone and boundary conditions (see

Defining Transient Cell Zone and Boundary Conditions (p. )) and point properties for particle injections

(see Point Properties for Transient Injections (p. )).

There are two profile format options:

.... Standard Profiles

.... CSV Profiles

The format of the profile files is fairly simple. The file can contain an arbitrary number of profiles. Each

profile consists of a header that specifies the profile name, profile type (point, line, mesh, radial,

or axial), and number of defining points, and is followed by an arbitrary number of named “fields”.

Some of these fields contain the coordinate points and the rest contain boundary data.

Important

Keep profile names to  characters or less. If the profile name contains more than

characters, Fluent truncates the name to the first  characters.

All quantities, including coordinate values, must be specified in SI units because ANSYS

Fluent does not perform unit conversion when reading profile files.

Parentheses are used to delimit profiles and the fields within the profiles. Any combination of tabs,

spaces, and newlines can be used to separate elements.

Important

In the general format description below,“ |” indicates that you should input only one of

the items separated by |’s and “ ...” indicates a continuation of the list.

((profile1-name point|line|radial n)

(field1-name a1 a2 ... an)

(field2-name b1 b2 ... bn)

.

.

.

(fieldf-name f1 f2 ... fn))

((profile2-name mesh m n)

(field1-name  a11 a12 ... a1n

a21 a22 ... a2n

.

.

.

am1 am2 ... amn)

.

.

.

(fieldf-name   f11  f12 ... f1n

f21  f22 ... f2n

.

.

.

fm1 fm2 ... fmn))

Profile names must have all lowercase letters (for example, name). Uppercase letters in profile names

are not acceptable. Each profile of type point, line, and mesh must contain fields with names x,

y, and, for 3D, z. Each profile of type radial must contain a field with name r. Each profile of type

axial must contain a field with name z. The rest of the names are arbitrary, but must be valid

Scheme symbols. For compatibility with old-style profile files, if the profile type is missing, point is

assumed.

..... Example

A typical usage of a profile file is to specify the profile of the boundary layer at an inlet. For a com-

pressible flow calculation, this will be done using profiles of total pressure,

, and . For an incom-

pressible flow, it might be preferable to specify the inlet value of streamwise velocity, together with

and .

Profiles

Below is an example of a profile file that does this:

((turb-prof point )

(x

and .

Profiles

(x

.00000E+  .00000E+  .00000E+  .00000E+

.00000E+  .00000E+  .00000E+  .00000E+ )

(y

.06443E-  .19485E-  .33020E-  .47418E-

.90494E-  .31222E-  .84519E-  .57471E- )

(u

.47866E+  .59870E+  .05731E+  .40079E+

.01674E+  .01656E+  .01637E+  .01616E+ )

(tke

.93228E-  .19247E-  .32680E-  .93642E-

.89414E-  .89666E-  .90015E-  .90478E- )

(eps

.27713E+  .04399E+  .31187E+  .21535E+

.78365E-  .79056E-  .80001E-  .81265E- )

)

CSV profiles are compatible with spreadsheets and are available for both reading and writing in Fluent.

Many profile types can be written in CSV format, including:

Radial

Axial

Point (X,Y, Z)

Transient

Transient-Periodic

If writing a profile using the Write Profile dialog box, you can save the profile in CSV format by saving

with a .csv extension.

Formatting Rules:

CSV profiles must be setup so they can be read and interpreted correctly in Fluent:

. The profile file must contain the section identifiers shown in Table . : CSV Profile Section Identifiers

(p. ).These identifiers must be used in the order, [Name] then [Data].

Table . : CSV Profile Section Identifiers

Remark

Section Identifiers

Next line should have the profile name. Note- if

the profile name has space characters, they will be

replaced with '_' (space character is not allowed).

[Name]

Data values begin on the next line.

[Data]

. After the [Data] identifier you must label the type of data that you are providing; refer to

Table . : Profile Types and the Corresponding Required Field Labels (p. ) for the correct labels. If

Fluent does not find one of the expected labels, the profile read will fail.

Table . : Profile Types and the Corresponding Required Field Labels

Required Field Label

Profile Type

radius

radial

axis

axial

X, Y, Z

point

time, angle

transient

time-periodic, angle-periodic

transient-periodic

Important

The following labels are reserved for X-axis functions: x, y, z, r, time, and angle. If

your file contains fields labeled with any of these reserved names, then those fields

will be treated as X-axis functions. For fields to be considered as Y-axis functions, you

must use names that are not reserved for X-axis functions.

. If there is an unsupported section identifier, Fluent ignores the section and looks for the [Name] and

[Data] section identifiers.

. Multiple profiles may be included in a single file.

Important

Only use commas as value separators. Space characters should not be used as they will confuse

external spreadsheet applications.

Only SI values are supported. Quantities cannot be entered with units.

CSV Profile File Examples

A file containing one profile:

[Name]

outlet

[Data]

x,y,z,x-velocity

.,.,,.

.,-.,,.

.,-.,,    .

.,.,,.

.,.,,.

.,.,,.

A file containing two profiles, the first one is spatial (steady-state) and the second is transient.

[Name]

outlet

Profiles

[Data]

.,.,,.

.,-.,,.

[Name]

transient-temperature

[Data]

time,temperature

.,

.,

.,

The procedure for using a profile to define a particular cell zone or boundary condition is outlined

below.

. Create a file that contains the desired profile, following the format described in Profile File Formats (p. ).

below.

. Read the profile using the Read... button in the Profiles Dialog Box (p. ) (Figure . :The Profiles Dialog

Box (p. ))

or the File/Read/Profile... ribbon tab item.

Setup →

Cell Zone Conditions → Profiles...

Setup →

Boundary Conditions → Profiles...

Note that if you use the Profiles dialog box to read a file, and a profile in the file has the same

name as an existing profile, the old profile will be overwritten.

. If it is a point profile, you can choose the method of interpolation using the Profiles dialog box (Fig-

ure . :The Profiles Dialog Box (p. )):

Setup →

Setup →

Select the point profile in the Profile selection list. Then select one of the three choices in the In-

terpolation Method list and click the Apply button. The three choices include:

Constant

This method is zeroth-order interpolation. For each cell face at the boundary, the solver uses the

value from the profile file located closest to the cell. Therefore, the accuracy of the interpolated

profile will be affected by the density of the data points in your profile file. This is the default

interpolation method for point profiles.

Inverse Distance

This method assigns a value to each cell face at the boundary based on weighted contributions

from the values in the profile file. The weighting factor is inversely proportional to the distance

between the profile point and the cell face center.

Least Squares

This method assigns values to the cell faces at the boundary through a first-order interpolation

method that tries to minimizes the sum of the squares of the offsets (residuals) between the

profile data points and the cell face centers. The least squares solution is found using Singular

Value Decomposition (SVD).

Note

The Inverse Distance and Least Squares profile interpolation methods are not applicable

when a profile is attached to cell zones.

For information about the interpolation methods employed for other profile types (that is, line,

mesh, radial, or axial profiles), see Profile Specification Types (p. ).

. You can attach a profile to a reference frame so that the profile will rotate according to the reference

frame.This can be used to model the clocking effect of a rotor on a stator, for example. Under Reference

Frames, select the reference frame to attach the chosen profile to.

. In the boundary conditions dialog boxes (for example, the Velocity Inlet and Pressure Inlet dialog boxes),

the fields defined in the profile file (and those defined in any other profile file that you have read in) will

appear in the drop-down list to the right of or below each parameter for which profile specification is al-

lowed.To use a particular profile, select it in the appropriate list.

. Initialize the solution to interpolate the profile.

Note

You can use a profile file or the DEFINE_PROFILE user-defined function to specify volu-

metric source terms. If you specify the source terms with a profile, you will not have access

to the central coefficient of the equations solved in order to linearize the source term. You

will need to use a user-defined function to do this.

For more information on UDFs, refer to the Fluent Customization Manual.

.... Checking and Deleting Profiles

Each profile file contains one or more profiles, and each profile has one or more fields defined in it.

Once you have read in a profile file, you can check which fields are defined in each profile, and you

can also delete a particular profile. These tasks are accomplished in the Profiles Dialog Box (p. )

(Figure . : The Profiles Dialog Box (p. )).

Setup →

Setup →

Profiles

Figure . : The Profiles Dialog Box

To check which fields are defined in a particular profile, select the profile name in the Profile list. The

available fields in that file will be displayed in the Fields list. In Figure . : The Profiles Dialog

Box (p. ), the profile fields from the profile file of Example (p. ) are shown.

To delete a profile, select it in the Profile list and click the Delete button. When a profile is deleted,

all fields defined in it will be removed from the Fields list.

Important

If you are deleting an existing profile to replace it with a new profile, use the following

.

Delete the existing profile.

.

Change the parameters defined by the existing profile to Constant.

.

Read the new profile and apply as desired.

....Viewing Profile Data

The Plots task page options allow you to generate XY plots of data related to profiles. You can plot

the original data points from the profile file you have read into ANSYS Fluent, or you can plot the

values assigned to the cell faces on the boundary after the profile file has been interpolated. See XY

Plots of Profiles (p. ) for the steps to generate these plots.

You have the additional option of viewing the parameters) using the Plot or the Contours options.

Note that these display options do not allow you to plot the actual values of the cell faces (as is done

with the Interpolated Data option), because they interpolate the values stored in the adjacent cells.

To view the boundary condition parameters you must first read in the profile, save a boundary con-

dition with a profile field selected as a parameter, and initialize the flow solution. Then you can view

the surface data as follows:

For 2D calculations, open the Solution XY Plot dialog box. Select the appropriate boundary zone in the

Surfaces list, the variable of interest in the Y Axis Function drop-down list, and the desired Plot Direction.

Ensure that the Node Values check button is turned on, and then click Plot.You should then see the

profile plotted. If the data plotted does not agree with your specified profile, this means that there is an

error in the profile file.

For 3D calculations, use the Contours dialog box to display contours on the appropriate boundary zone

surface.The Node Values check button must be turned on in order for you to view the profile data. If the

data shown in the contour plot does not agree with your specified profile, this means that there is an error

in the profile file.

.... Example

In Figure . : Example of Using Profiles as Boundary Conditions (p. ), profiles are used to specify

the gauge total pressure and the x, y, z flow direction components at a pressure inlet boundary.

Figure . : Example of Using Profiles as Boundary Conditions

For 3D cases only, ANSYS Fluent allows you to change the orientation of an existing profile so that it

can be used at a boundary positioned arbitrarily in space. This allows you, for example, to take exper-

imental data for an inlet with one orientation and apply it to an inlet in your model that has a different

spatial orientation. Note that ANSYS Fluent assumes that the profile and the boundary are planar.

Profiles

.... Steps for Changing the Profile Orientation

The procedure for orienting the profile data in the principal directions of a boundary is outlined below:

. Define and read the profile as described in Using Profiles (p. ).

. In the Profiles Dialog Box (p. ), select the profile in the Profile list, and then click the Orient... button.

This will open the Orient Profile Dialog Box (p. ) (Figure . :The Orient Profile Dialog Box (p. )).

Figure . : The Orient Profile Dialog Box

. In the Orient Profile dialog box, enter the name of the new profile you want to create in the New Profile

box.

. Specify the number of fields you want to create using the up/down arrows next to the New Fields box.

The number of new fields is equal to the number of vectors and scalars to be defined plus  (for the co-

ordinates).

. Define the coordinate field.

a.

Enter the names of the three coordinates ( ,

, ) in the first row under New Field Names.

Important

Ensure that the coordinates are named ,

, and  only. Do not use any other

a.

Important

names or upper case letters in this field.

b. Select the appropriate local coordinate fields for ,

, and  from the drop-down lists under Compute

From.... (A selection of  indicates that the coordinate does not exist in the original profile; that is,

the original profile was defined in 2D.)

. Define the vector fields in the new profile.

a.

Enter the names of the  components in the directions of the coordinate axes of the boundary under

New Field Names.

Important

Do not use upper case letters in these fields.

b. Select the names of the  components of the vector in the local ,

, and  directions of the profile

from the drop-down lists under Compute From....

. Define the scalar fields in the new profile.

a.

Enter the name of the scalar in the first column under New Field Names.

Important

b. Click the button under Treat as Scalar Quantity in the same row.

c.

Select the name of the scalar in the corresponding drop-down list under Compute From....

. Under Orient To..., specify the rotational matrix

under the Rotation Matrix [RM].The rotational

matrix used here is based on Euler angles ( ,

, and ) that define an orthogonal system

as the

result of the three successive rotations from the original system

.That is,

(.)

(.)

where C, B, and A are the successive rotations around the ,

, and  axes, respectively.

Rotation around the  axis:

(.)

(.)

Profiles

(.)

(.)

(.)

Profiles

(.)

. Under Orient To..., specify the Direction Vector.The Direction Vector is the vector that translates a

profile to the new position, and is defined between the centers of the profile fields.

Important

Note that depending on your case, it may be necessary to perform only a rotation, only

a translation, or a combination of a translation and a rotation.

. Click the Create button in the Orient Profile dialog box, and your new profile will be created. Its name,

which you entered in the New Profile box, will now appear in the Profiles dialog box and will be available

for use at the desired boundary.

.... Profile Orienting Example

Consider the domain with a square inlet and outlet, shown in Figure . : Scalar Profile at the Out-

let (p. ). A scalar profile at the outlet is written out to a profile file. The purpose of this example is

to impose this outlet profile on the inlet boundary via a ° rotation about the  axis. However, the

rotation will locate the profile away from the inlet boundary. To align the profile to the inlet boundary,

a translation via a directional vector must be performed.

Figure . : Scalar Profile at the Outlet

The problem is shown schematically in Figure . : Problem Specification (p. ).

is the scalar

profile of the outlet.

is the image of the

rotated ° around the  axis. In this example, since

, then

, where  is the identity matrix, and the rotation matrix is

(.)

To overlay the outlet profile on the inlet boundary, a translation will be performed.

, then

(.)

To overlay the outlet profile on the inlet boundary, a translation will be performed. The directional

vector is the vector that translates

to

. In this example, the directional vector is

.

The appropriate inputs for the Orient Profile dialog box are shown in Figure . : The Orient Profile

Dialog Box (p. ).

Note that if the profile being imposed on the inlet boundary was due to a rotation of -° about the

axis, then the rotational matrix

must be found for

and

, and a new directional

vector must be found to align the profile to the boundary.

Profiles

Figure . : Problem Specification

In many turbomachinery cases, a profile can be obtained from an initial small-scale simulation (often

one passage but sometimes more) and then applied to a larger, often full  degree, simulation.

Replicating a profile enables you to copy the initial profile periodically for use in a larger simulation.

.... Steps for Replicating a Profile

The procedure for replicating the profile data periodically is outlined below:

. Open the Profiles dialog box.

Physics → Zones → Profiles...

. Select the profile to replicate and click Replicate... to open the Replicate Profile dialog box (Fig-

ure . :The Replicate Profile Dialog Box (p. )).

Figure . : The Replicate Profile Dialog Box

a.

Enter a name in the New Profile field (for the expanded profile name).

b. Specify the number of fields you want to create using the up/down arrows next to the New Fields

a.

box.The number of new fields is equal to the number of vectors and scalars to be defined plus

(including the coordinates).

c.

Define the coordinate field.

i.

Enter the names of the three coordinates (x, y, z) in the first row under New Field Names.

Important

Ensure that the coordinates are named x, y, and z only. Do not use any other

ii.

Select the appropriate local coordinate fields for x, y, and z from the drop-down lists under

Compute From.... (A selection of  indicates that the coordinate does not exist in the original

profile; that is, the original profile was defined in 2D.)

d. Define the vector fields in the new profile.

Profiles

i.

Enter the names of the  components in the directions of the coordinate axes under New Field

Names.

Important

ii.

Select the names of the  components of the vector in the local coordinates of the profile from

the drop-down lists under Compute From....

e. Define the scalar fields in the new profile.

i.

Important

ii.

Select Treat as Scalar Quantity in the same row.

iii. Select the name of the scalar in the corresponding drop-down list under Compute From....

. Specify the replication settings in the Current Profile Definitions group box.

a.

If you are creating a full  degree profile, select Full  deg.. Fluent automatically determines

a.

the number of copies of the original profile that are needed to make the full  degree profile based

on the other information you specify.

b. If you did not select Full  deg., you must specify the Number of copies to manually determine

how many copies of the original profile are created.

c.

The Number of sectors in  deg. is the number of periodic sections, based on the original profile,

that are present in  degrees.

d. The Number of sectors in profile is the number of periodic sections in the original profile.

e. The Calculated angle is for display only and is the angle occupied by the original profile.When using

the Full  deg. option, you can determine the number of copies that are created by dividing

by the Calculated angle.

f.

Specify the Rotation-Axis Direction.This is the X, Y, and Z components of the axis about which the

selected profile is replicated.

. Click the Create button in the Replicate Profile dialog box, and your new profile will be created. Its

name, which you entered in the New Profile box, will now appear in the Profiles dialog box and will be

available for use at the desired boundary.

There are three ways you can specify transient cell zone and boundary conditions:

transient profile with a format similar to the standard profiles described in Profiles (p. )

transient profile in a tabular format

transient profile in comma separated values (CSV) format, as described in CSV Profiles (p. ).

Important

Important

For both methods, the cell zone or boundary condition will vary only in time; it must be

spatially uniform. However, if the in-cylinder model is activated (In-Cylinder Settings (p. )),

then you have the option to use the crank angle instead of time. Crank angles can be in-

cluded in transient tables as well as transient profiles, in a similar fashion to time. Examples

of transient profiles and transient tables in crank angle can be found in the sections that

follow.

For information about boundary profiles, refer to Reading and Writing Profile Files (p. ).

.... Standard Transient Profiles

The format of the standard transient profile file (based on the profiles described in Profiles (p. ))

is

((profile-name transient n periodic?)

(field_name- a1 a2 a3 .... an)

(field_name- b1 b2 b3 .... bn)

.

.

.

.

(field_name-r r1 r2 r3 .... rn))

The profile name as well as the field names have to be shorter than  characters. One of the

field_name s should be used for the time field, and the time field section must be in ascending

order. n is the number of entries per field. The periodic? entry indicates whether or not the profile

is time-periodic. Set it to  for a time-periodic profile, or  if the profile is not time-periodic.

An example is shown below:

((sampleprofile transient  )

(time

)

(u

)

)

This example demonstrates the use of crank angle in a transient profile

((example transient  )

(angle

.000000e+ .800000e+ .600000e+)

(temperature

Profiles

.000000e+ .000000e+ .000000e+)

)

Important

(angle

Profiles

)

Important

Fluent does not perform unit conversion when reading profile files. Also, profile names

must have all lowercase letters (for example, name). Uppercase letters in profile names are

not acceptable.

You can read this file into ANSYS Fluent using the Profiles Dialog Box (p. ) or the File/Read/Profile...

Setup →

Setup →

See Using Profiles (p. ) for details.

....Tabular Transient Profiles

The format of the tabular transient profile file is

profile-name n_field n_data periodic?

field-name- field-name- field-name- .... field-name-n_field

v--  v--... ... ... ... v-n_field-

.

.

.

.

.

v--n_data v--n_data ... ... ... ... v-n_field-n_data

The first field name (for example field-name-) should be used for the time field, and the time

field section, which represents the flow time, must be in ascending order. The periodic? entry in-

dicates whether or not the profile is time-periodic. Set it to  for a time-periodic profile, or  if the

profile is not time-periodic.

sampletabprofile

time u

This file defines the same transient profile as the standard profile example above.

If the periodicity is set to , then n_data must be the number that closes one period.

periodtabprofile

time u

The following example uses crank angle instead of time:

example

angle temperature

Important

time u

example

Important

All quantities, including coordinate values, must be specified in SI units because ANSYS Flu-

ent does not perform unit conversion when reading profile files. Also, profile names must have

all lowercase letters (for example, name). Uppercase letters in profile names are not acceptable.

When choosing the field names, spaces or parentheses should not be included.

Some file formats may not be read into Fluent correctly (for example, UCS-). If your file is not

read correctly, copy the contents into a text editor (Notepad++/VIM/Notepad) and save it.This

updated version of your profile is now readable in Fluent.

You can read this file into ANSYS Fluent using the read-transient-table text command.

file → read-transient-table

After reading the table into ANSYS Fluent, the profile will be listed in the Profiles Dialog Box (p. )

and can be used in the same way as a boundary profile. See Using Profiles (p. ) for details.

.... Profiles for Moving and Deforming Meshes

You can use profiles to specify position, velocity, and angular velocity. There are two different valid

profile formats for moving and deforming mesh cases.

.

.

.

.

.

and

.

.

.

.

Profiles

and

.

.

.

.

Profiles

You must use the appropriate variable nomenclature when writing your profile so that Fluent can

properly interpret your inputs. For position, use x, y, and z. For specifying velocity, use v_x, v_y,

and v_z. Similarly, for angular velocity, use omega_x, omega_y, and omega_z.

GT-POWER users can define time-dependent boundary conditions in ANSYS Fluent based on information

from GT-POWER. During the ANSYS Fluent simulation, ANSYS Fluent and GT-POWER are coupled together

and information about the boundary conditions at each time step is transferred between them.

... Requirements and Restrictions

... User Inputs

...Torque-Speed Coupling with GT-POWER

Note the following requirements and restrictions for the GT-POWER coupling:

The flow must be unsteady.

The compressible ideal gas law must be used for density.

Each boundary zone for which you plan to define conditions using GT-POWER must be a boundary of one

of the following types:

– velocity inlet

– mass-flow inlet

– pressure inlet

– pressure outlet

– wall (for details, see Torque-Speed Coupling with GT-POWER (p. ))

Also, a maximum of  boundary zones can be coupled to GT-POWER.

Fluent checks the area of the 1D coupled boundary as calculated by Fluent and GT-POWER to ensure the

calculated areas differ by no more than %.When the difference is more than %, Fluent stops with an

error message and displays the two areas.

If a mass-flow inlet or pressure inlet is coupled to GT-POWER, you must select Normal to Boundary as the

Direction Specification Method in the Mass-Flow Inlet or Pressure Inlet dialog box. For a velocity inlet,

you must select Magnitude, Normal to Boundary as the Velocity Specification Method in the Velocity

Inlet dialog box.

The mass flow specification method in the Mass-Flow Inlet boundary has to always be Mass Flux and not

Mass Flow Rate when coupling with GTPower.

Boundary conditions for the following variables can be obtained from GT-POWER:

– velocity

– temperature

– pressure

– density

– species mass fractions

–

and  (Note that it is recommended that you define these conditions in ANSYS Fluent yourself, rather

than using the data provided by GT-POWER, since the GT-POWER values are based on a 1D model.)

Make sure that the material properties you set in ANSYS Fluent are the same as those used in GT-POWER,

so that the boundary conditions will be valid for your coupled simulation.

If your model includes species, make sure that the name of each species in GT-POWER corresponds to the

Chemical Formula for that species material in the Materials dialog box. Also, recall that ANSYS Fluent can

handle a maximum of  species.

You can install the GT-POWER libraries in a directory other than the default location. If the GT-POWER lib-

raries are loaded into a non-default location, you need to set the following environment variables:

– Fluent_GTIHOME — the GTI installation directory where GT-POWER is installed

– Fluent_GTIVERSION — the current version of the GTI installation

Important

GTI is not backwards compatible.

Important

The procedure for setting up the GT-POWER coupling in ANSYS Fluent is presented below.

. Read in the mesh file and define the models, materials, and boundary zone types (but not the actual

boundary conditions), noting the requirements and restrictions listed in Requirements and Restric-

. Specify the location of the GT-POWER data and have ANSYS Fluent use them to generate user-defined

functions for the relevant boundary conditions (using the 1D Simulation Library Dialog Box (p. ), shown

in Figure . :The 1D Simulation Library Dialog Box (p. )).

User Defined → Model Specific → 1D Coupling...

Coupling Boundary Conditions with GT-POWER

Figure . : The 1D Simulation Library Dialog Box

a.

Select GTpower in the 1D Library drop-down list.

b. Specify the name of the GT-POWER input file in the 1D Input File Name field.

c.

Click the Start button.

When you click Start, GT-POWER will start up and ANSYS Fluent user-defined functions for each

boundary in the input file will be generated.

. Set boundary conditions for all zones. For flow boundaries for which you are using GT-POWER data, select

the appropriate UDFs as the conditions.

Important

Note that you must select the same UDF for all conditions at a particular boundary zone

(as shown, for example, in Figure . : Using GT-POWER Data for Boundary Condi-

tions (p. )); this UDF contains all of the conditions at that boundary.

Figure . : Using GT-POWER Data for Boundary Conditions

. If you plan to continue the simulation at a later time, starting from the final data file of the current simu-

lation, specify how often you want to have the case and data files saved automatically.

Solution →

Calculation Activities (Autosave Case/Data) → Edit...

To use a GT-POWER restart file to restart an ANSYS Fluent calculation, you must edit the GT-POWER

input data file. See the GT-POWER User’s Guide for instructions.

. Continue the problem setup and calculate a solution in the usual manner.

Torque-speed coupling with GT-POWER is a unique case in which Fluent receives shaft speed from

GT-POWER and returns torque. The procedure differs from the typical coupling between GT-Power

and Fluent, and is as follows:

Important

You must be using GT-POWER v2017. or greater to perform torque-speed coupling with

. Complete steps  and  in the above section on User Inputs (p. ).The .dat file should have at least

one turbo-machine exposed to complete the coupling.

. Enable Frame Motion in the cell zone that is receiving shaft speed from GT-Power.You must also select

the appropriate UDF for Rotational Velocity.The UDF must correspond to the turbo-machine exposed

from GT-POWER ("turbine", in the example shown below).

Figure . : Cell Zone Conditions for Torque-Speed Coupling with GT-POWER

. Specify a Wall boundary on which the torque is calculated and transferred to GT-POWER.The following

requirements apply:

The wall boundary must be attached to the rotating cell zone from step , to receive the shaft speed

from GT-POWER.

The name of the wall boundary must be the same as the turbo-machine it is coupled with ("turbine",

in the case presented above).

During the solution, shaft speed is obtained from GT-POWER at every time-step, with Fluent calculating

and returning torque within each time-step as well.

WAVE users can define time-dependent boundary conditions in ANSYS Fluent based on information

from WAVE. During the ANSYS Fluent simulation, ANSYS Fluent and WAVE are coupled together and

information about the boundary conditions at each time step is transferred between them.

Note the following requirements and restrictions for the WAVE coupling:

WAVE must be installed and licensed.

There are always five species that must be modeled in ANSYS Fluent just as they are defined in WAVE (F1,

F2, F3, F4, and F5). It is recommended that realistic material properties be assigned to each of the five

species.

Each boundary zone for which you plan to define conditions using WAVE must be a flow boundary of one

Also, a maximum of  boundary zones can be coupled to WAVE.

If a mass-flow inlet or pressure inlet is coupled to WAVE, you must select Normal to Boundary as the Dir-

ection Specification Method in the Mass-Flow Inlet or Pressure Inlet Dialog Box. For a velocity inlet,

Inlet Dialog Box.

Boundary conditions for the following variables can be obtained from WAVE:

– velocity

– pressure

Coupling Boundary Conditions with WAVE

– density

–

and  (Note that you are required to define these conditions in ANSYS Fluent yourself, since WAVE

does not calculate them.)

Make sure that the material properties you set in ANSYS Fluent are the same as those used in WAVE, so

that the boundary conditions will be valid for your coupled simulation.

If your model includes species, make sure that the name of each species in WAVE corresponds to the

Chemical Formula for that species material in the Create/Edit Materials dialog box. Also, recall that ANSYS

Fluent can handle a maximum of  species.

The procedure for setting up the WAVE coupling in ANSYS Fluent is presented below.

. Read in the mesh file and define the models, materials, and boundary zone types.

. Specify the location of the WAVE data and have ANSYS Fluent use them to generate user-defined functions

for the relevant boundary conditions (using the 1D Simulation Library Dialog Box (p. ), shown in Fig-

ure . :The 1D Simulation Library Dialog Box with WAVE Selected (p. )).

Figure . : The 1D Simulation Library Dialog Box with WAVE Selected

a.

Select WAVE in the 1D Library drop-down list.

b. Specify the name of the WAVE input file in the 1D Input File Name field.

c.

a.

c.

When you click Start, WAVE will start up and ANSYS Fluent user-defined functions for each

. Set boundary conditions for all zones. For flow boundaries for which you are using WAVE data, select the

appropriate UDFs as the conditions.

Important

(as shown, for example, in Figure . : Using WAVE Data for Boundary Conditions (p. ));

this UDF contains all of the conditions at that boundary.

Figure . : Using WAVE Data for Boundary Conditions

. If you plan to continue the simulation at a later time, restarting from the final data file of the current

simulation, you need to instruct both ANSYS Fluent and WAVE how often that you want to automatically

save your data.You should instruct ANSYS Fluent to automatically save case and data files at specified

intervals using the autosave feature.

Solution → Calculation Activities → Autosave

On

In addition, you should instruct WAVE as to how often it should generate its own restart files. See

the WAVE User's Guide for instructions on this feature.

Important

To use the restart feature, the time interval for writing data files must be set to the same

value in both ANSYS Fluent and WAVE. For example, if ANSYS Fluent has set the autosave

feature to , then WAVE must also set the restart file write frequency to  as well.

Chapter : Physical Properties

This chapter describes how to define materials, the physical equations used to compute material

properties, and the methods you can use for each property input. Each property is described in detail

in the following sections. If you are using one of the general multiphase models (VOF, mixture, or Eu-

lerian), see Defining the Phases (p. ) for information about how to define the individual phases and

their material properties.

.. Defining Materials

.. Defining Properties Using Temperature-Dependent Functions

.. Density

..Viscosity

..Thermal Conductivity

.. User-Defined Scalar (UDS) Diffusivity

.. Specific Heat Capacity

.. Radiation Properties

.. Mass Diffusion Coefficients

.. Standard State Enthalpies

.. Standard State Entropies

.. Unburnt Thermal Diffusivity

.. Kinetic Theory Parameters

.. Operating Pressure

.. Reference Pressure Location

.. Real Gas Models

An important step in the setup of the model is to define the materials and their physical properties.

Material properties are defined using either the Materials Task Page (p. ) or the Materials tree branch,

where you can enter values for the properties that are relevant to the problem scope you have defined

in the Models Task Page (p. ). These properties may include the following:

density and/or molecular weights

viscosity

heat capacity

thermal conductivity

UDS diffusion coefficients

mass diffusion coefficients

standard state enthalpies

kinetic theory parameters

Properties may be temperature-dependent and/or composition-dependent, with temperature dependence

based on a polynomial, piecewise-linear, or piecewise-polynomial function and individual component

properties either defined by you or computed via kinetic theory.

The Materials Task Page (p. ) will show the properties that need to be defined for the active physical

models. If any property you define requires the energy equation to be solved (for example, ideal gas

law for density, temperature-dependent profile for viscosity), ANSYS Fluent will automatically enable

the energy equation. Then you have to define the thermal boundary conditions and other parameters

yourself.

... Physical Properties for Solid Materials

... Material Types and Databases

... Using the Create/Edit Materials Dialog Box

... Using a User-Defined Materials Database

For solid materials, only density, thermal conductivity, and heat capacity are defined. If you are mod-

eling semi-transparent media, then radiation properties are also defined. You can specify a constant

value, a temperature-dependent function, or a user-defined function for thermal conductivity; a constant

value or temperature-dependent function for heat capacity; and a constant value for density.

If you are using the pressure-based solver, density and heat capacity for a solid material are not required

unless you are modeling transient flow or moving solid zones. Heat capacity will appear in the list of

solid properties for steady flows as well. The value will be used just for postprocessing enthalpy; not

in the calculation.

In ANSYS Fluent, you can define six types of materials: fluids, solids, mixtures, combusting-particles,

droplet-particles, and inert-particles. Physical properties of fluids and solids are associated with named

material; these materials are then assigned as boundary conditions for zones.

When you model species transport, define a mixture material, consisting of the various species involved

in the problem. Properties will be defined for the mixture, as well as for the constituent species, which

are fluid materials. The mixture material concept is discussed in detail in Mixture Materials (p. ).

Combusting-particles, droplet-particles, and inert-particles are available for the discrete-phase model,

as described in The Concept of Discrete-Phase Materials (p. ).

ANSYS Fluent provides a built-in global database of approximately  predefined materials along

with their properties and default values for each property. To define a material in the problem setup,

you can copy materials from this global (site-wide) database and use the default properties or define

new materials by editing their properties. The ANSYS Fluent materials database is located in the fol-

lowing file:

path /ansys_inc/v195/fluent/fluent19../cortex/lib/propdb.scm

where path is the directory in which you installed ANSYS Fluent.

Physical Properties

In addition to using the ANSYS Fluent material database, you can also create your own database and

materials, and use it to define the materials in your problem setup. See Using a User-Defined Materials

Database (p. ) for information about creating and using user-defined custom material databases.

Important

All the materials in your local materials list will be saved in the case file (when you write

one). The materials specified by you will be available to you if you read this case file into a

new solver session.

The Create/Edit Materials Dialog Box (p. ) allows you to define the materials and their properties in

your problem setup using either the Fluent Database or a User-Defined Database. It enables you to

copy materials from a database, create new materials, and modify material properties.

These generic functions are described in this section. The inputs for temperature-dependent properties

are explained in Defining Properties Using Temperature-Dependent Functions (p. ). The specific inputs

for each material property are discussed in the remaining sections of this chapter.

The Create/Edit Materials Dialog Box (p. ) can be accessed in one of two ways:

Through the Materials task page.

Setup →

Materials

Defining Materials

Figure . : The Materials Task Page

Through the material types (Fluid, Solid, and so on) and defined in the case materials under Materials in

the tree.

For example, if you want to create a new fluid material you can access the Create/Edit Materials

dialog box as follows:

Setup → Materials → Fluid

New...

Figure . : The Materials Branch in the Outline View

By default, your local materials list will include a single fluid material (air) and a single solid material

New...

(aluminum). If the fluid involved in your problem is air, you can use the default properties for air or

modify the properties. If the fluid in your problem is water, you can either copy water from the ANSYS

Fluent database or create a new “water” material from scratch. If you copy water from the database,

you can still make modifications to the properties of your local copy of water. See the following sections

for detailed information on how to change material properties.

Mixture materials will not exist in your local list unless you have enabled species transport (see Modeling

Species Transport and Finite-Rate Chemistry (p. )). Similarly, inert, droplet, and combusting particle

materials will not be available unless you have created a discrete phase injection of these particle types

(see Modeling Discrete Phase (p. )). When a mixture material is copied from the database, all of its

constituent fluid materials (species) will automatically be copied over as well.

.... Modifying Properties of an Existing Material

Probably, the most common operation you will perform in the Create/Edit Materials Dialog Box (p. )

is the modification of properties for an existing material. The steps for this procedure are as follows:

. In the Materials Task Page (p. ), select the material you want to modify and click the Create/Edit...

button. (You can also right-click the material in the tree and select Edit... from the material submenu.)

. In the Create/Edit Materials Dialog Box (p. ) select the type of material (fluid, solid, and so on) in the

Material Type drop-down list.

. Choose the material for which you want to modify properties, in the Fluent Fluid Materials drop-down

list, Fluent Solid Materials list, or other similarly named list.The name of the list will be the same as the

material type you selected in the previous step.

. Make the required changes to the properties listed in the Properties section of the dialog box.You can

use the scroll bar to the right of the Properties section to scroll through the listed items.

. Click the Change/Create button to change the properties of the selected material to your new property

settings.

To change the properties of an additional material, repeat the process described above. Click the

Change/Create button after making changes to the properties for each material.

.... Renaming an Existing Material

Each material is identified by a name and a chemical formula (if one exists). You can change the name

of a material, but not its chemical formula (unless you are creating a new material). The procedure

for renaming a material is as follows:

. In the Materials Task Page (p. ), select the material you want to rename and click the Create/Edit...

. In the Create/Edit Materials Dialog Box (p. ), choose the material for which you want to modify prop-

erties, in the Fluent Fluid Materials list, Fluent Solid Materials list, or other similarly named list.The

name of the list will be the same as the material type you selected in the previous step.

. Enter the new name in the Name field at the top of the Create/Edit Materials Dialog Box (p. ).

Important

The maximum character length you can enter in the Name field is . If you enter a

material name that is more than  characters long, ANSYS Fluent will print an error

message in the console window.

. Click the Change/Create button.

A Question Dialog Box (p. ) will appear, asking you if the original material should be overwritten.

If you are renaming the original material, click Yes to overwrite it. If you were creating a new

material, click No to retain the original material.

To rename another material, repeat the process described above. Click the Change/Create button

after renaming each material.

.... Copying Materials from the ANSYS Fluent Database

The global (site-wide) materials database contains many commonly used fluid, solid, and mixture

materials, with property data from several different sources  [] (p. ), [] (p. ), [] (p. ),

[] (p. ). To use one of these materials in your problem, copy it from the ANSYS Fluent database

to your local materials list. The procedure for copying a material is as follows:

. Click the Fluent Database... button in the Create/Edit Materials Dialog Box (p. ) to open the Fluent

Database Materials Dialog Box (p. ) (Figure . : Fluent Database Materials Dialog Box (p. )).

Figure . : Fluent Database Materials Dialog Box

. Select the type of material (fluid, solid, and so on) in the Material Type drop-down list.

. In the Fluent Fluid Materials list, Fluent Solid Materials list, or other similarly named list, choose the

materials you want to copy by clicking on them.The properties of the selected material will be displayed

in the Properties area.

. To check the material properties, use the scroll bar to the right of the Properties area to scroll through

the listed items. For some properties, temperature-dependent functions are available in addition to the

constant values. Select one of the function types in the drop-down list to the right of the property and

the relevant parameters will be displayed.You cannot edit these values, but the dialog boxes in which

they are displayed function in the same way as those used for setting temperature-dependent property

functions (Defining Properties Using Temperature-Dependent Functions (p. )).

The inactive buttons in the Fluent Database Materials Dialog Box (p. ) are operations that are ap-

plicable only for a user-defined database. These operations will be available when you click the User-

Defined Database... button in the Create/Edit Materials Dialog Box (p. ).

. Click Copy.

The materials and their properties will be downloaded from the database into your local list, and

your copy of properties will now be displayed in the Materials Task Page (p. ) and in the tree

under the appropriate material type.

. Close the Fluent Database Materials Dialog Box (p. ).

After copying a material from the database, you can modify its properties or change its name, as

described earlier in this section. The original material in the database will not be affected by any

changes made to your local copy of the material.

.... Creating a New Material

If the material you want to use is not available in the database, you can easily create a new material

for the local list. This material will be available for use only for the current problem and will not be

saved in the ANSYS Fluent database. The procedure for creating a new material is as follows:

. In the Materials Task Page (p. ), click the Create/Edit... button. (You can also right-click the correspond-

ing material type in the tree (Fluid, Solid, and so on) and select New... from the material type submenu.)

. Select the new material type (fluid, solid, and so on) in the Material Type drop-down list. It does not

matter which material is selected in the Fluent Fluid Materials, Fluent Solid Materials, or other similarly

named list.

. Enter the new material name in the Name field.

Important

. Set the material’s properties in the Properties area. If there are many properties listed, you may use the

scroll bar to the right of the Properties area to scroll through the listed items.

. Click the Change/Create button. A Question Dialog Box (p. ) will appear, asking you if the original

material should be overwritten.

a.

a.

Click No to retain the original material and add your new material to the list. A dialog box will appear

asking you to enter the chemical formula of your new material.

b. Click OK, enter the formula if it is known. Else, leave the formula blank and click OK. Select the

Change/Create button and answer the Question.

The Materials Task Page (p. ) and the Material tree branch will be updated to show the

new material name and chemical formula under the appropriate material type (Fluid, Solid,

or others).

.... Saving Materials and Properties

All the materials and properties in your local list are saved in the case file when it is written. If you

read this case file into a new solver session, all of your materials and properties will be available for

use in the new session.

.... Deleting a Material

If there are materials list that you no longer need, you can delete them in one of the following ways:

Using the Materials Task Page (p. ).

In the Materials Task Page (p. ), select the material to be deleted and click the Delete button at

the bottom of the Materials Task Page (p. ).

Using the tree.

Right-click the material in the tree and select Delete from the material submenu.

Using the Create/Edit Materials Dialog Box (p. ).

. From the Material Type drop-down list, select the type of material (fluid, solid, and so on).

. Select the material to be deleted from the Fluent Fluid Materials drop-down list, Fluent Solid Mater-

ials list, or other similarly named list.The list’s name will be the same as the material type you selected

in the previous step.

. Click the Delete button.

Deleting materials from your local list will have no effect on the materials contained in the global

database.

.... Changing the Order of the Materials List

By default, the materials in your local list and those in the database are listed alphabetically by name

(for example, air, atomic-oxygen (o), carbon-dioxide (co2)). If you prefer to list them alphabetically

by chemical formula, select the Chemical Formula option under Order Materials By. The example

materials listed, will now be in the order of: air, co2 (carbon-dioxide), o (atomic-oxygen). To change

back to the alphabetical listing by name, choose the Name option under Order Materials By.

You may specify the ordering method separately for the Create/Edit Materials Dialog Box (p. ) and

Fluent Database Materials Dialog Box (p. ). For example, you can order the database materials list

by name. Each dialog box has its own Order Materials By options.

In addition to the Fluent Database Materials Dialog Box (p. ), you can also use or create a user-

defined materials database using the User-Defined Database Materials Dialog Box (p. ). You can

browse and do the following:

select from existing user-defined databases

copy materials from a user-defined database

create a new database, create new materials

add them to the user-defined database

delete materials from the database

copy materials from a case to a user-defined database

view the database

The following sections will address each of these functionalities in detail.

.... Opening a User-Defined Database

In ANSYS Fluent, you can open databases of custom materials saved as .scm files and use them to

define the materials in your problem setup. The material data must be prepared in a specific format

as shown in the examples that follow.

Examples:

The prescribed format for saving material properties information is shown here for air and aluminum.

These files can be created in a text editor and saved with a .scm extension.

((air

fluid

(chemical-formula . #f)

(density (constant . .)

(premixed-combustion . ))

(specific-heat (constant . .))

(thermal-conductivity (constant . .))

(viscosity (constant . .7894e-)

(sutherland .7894e- . .)

(power-law .7894e- . .))

(molecular-weight (constant . .))

)

(aluminum

solid

(chemical-formula . al)

(density (constant . ))

(specific-heat (constant . ))

(formation-entropy (constant . .))

))

To select a user-defined database, click the User-Defined Database... button in the Create/Edit Ma-

terials Dialog Box (p. ). This will open the Open Database Dialog Box (p. ).

Figure . : Open Database Dialog Box

Click the Browse... button, select the database in The Select File Dialog Box (p. ) that opens and

click OK. Click OK in the Open Database Dialog Box (p. ) to open the User-Defined Database Ma-

terials Dialog Box (p. ).

....Viewing Materials in a User-Defined Database

When an existing user-defined database is opened, the materials present in the database are listed

in the User-Defined Database Materials Dialog Box (p. ). You can select the material type in the

Material Type drop-down list and the corresponding materials will appear in the User-Defined Fluid

Materials, User-Defined Solid Materials or other similarly named list. The name of the list will be

the same as the material type you selected.

Figure . : User-Defined Database Materials Dialog Box

The properties of the selected material will appear in the Properties section of the dialog box. This

dialog box is similar to the Fluent Database Materials Dialog Box (p. ) in function and operation.

.... Copying Materials from a User-Defined Database

The procedure for copying a material from a custom database is as follows:

. In the Create/Edit Materials Dialog Box (p. ), click the User-Defined Database... button and open the

database from which you want to copy the material.

. In the User-Defined Database Materials Dialog Box (p. ) of the selected database, select the type of

material (fluid, solid, and so on) in the Material Type drop-down list.

. In the User-Defined Fluid Materials list, User-Defined Solid Materials list, or other similarly named

list (the list’s name will be the same as the material type you selected in the previous step), choose the

materials you want to copy by clicking on them.The properties are displayed in the Properties area.

. If you want to check the material properties, use the scroll bar to the right of the Properties area to scroll

through the listed items.

. Click the Copy button.

The selected materials and their properties will be copied from the database into your local list,

and your copy of the properties will now be displayed in the Materials Task Page (p. ) and under

the Materials tree branch.

To copy all the materials from the database in one step, click the button (

) next to User-Defined

Materials title and click Copy.

If a material with the same name is already defined in the case, ANSYS Fluent will prompt you to

enter a new name and formula in the New Material Name Dialog Box (p. ). Enter a new name

and formula in the respective fields and click OK to make a local copy of the material.

Figure . : New Material Name Dialog Box

. Close the User-Defined Database Materials Dialog Box (p. ).

After copying a material from the database, you may modify its properties or change its name, as

described earlier in Using the Create/Edit Materials Dialog Box (p. ). The material in the database

will not be affected by any changes you make to your local copy of the material.

.... Copying Materials from the Case to a User-Defined Database

The procedure for copying a material to a custom database is as follows:

. In the Create/Edit Materials Dialog Box (p. ), click User-Defined Database....

. In the Open Database Dialog Box (p. ), select the database to which you want to copy the material. If

you want to create a new database, enter the name of the new database in the Database Name field

and click OK. A Question Dialog Box (p. ) will ask you to confirm if you want to create a new file. Click

Yes to confirm.

. In the User-Defined Database Materials Dialog Box (p. ), click Copy Materials From Case.....This will

open the Copy Case Material Dialog Box (p. ).

Figure . : Copy Case Material Dialog Box

a.

In the Copy Case Material Dialog Box (p. ), select the materials that you want to copy.

To select all the materials, click the shaded icon to the right of the Case Materials title. Clicking

on the unshaded icon will deselect the selections in the list.

b. Click Copy and close the dialog box.

Note

Do not copy materials one by one. This will result in previously copied materials

getting overwritten by the new ones. Instead, select all the materials to be copied

and click Copy.

You can modify the properties of an existing material and use the modified material in the problem

setup and save the modified material to the materials database.

database that you want to use.

a.

In the User-Defined Database Materials Dialog Box (p. ) of the selected database, select the type

of material (fluid, solid, and so on) in the Material Type drop-down list.

b. In the User-Defined Fluid Materials list, User-Defined Solid Materials list, or other similarly named

list (the name of the list will be the same as the material type you selected in the previous step), select

the material to be modified.

c.

Click Edit... to open the Material Properties Dialog Box (p. ).

i.

In the Materials Properties list, select the property to be modified and click Edit... to open the

Edit Property Methods Dialog Box (p. ).

ii.

i.

ii.

Select the method to be modified in the Material Properties list of the Edit Property Methods

Dialog Box (p. ) and click Edit... under Edit Properties, in order to modify the properties.

iii. Make the changes in the corresponding method dialog box and click OK.

iv. Click Apply in the Material Properties Dialog Box (p. ).

d. To use the modified material in the problem setup, click Copy in the User-Defined Database Materials

e. To save the modified material to the database, click Save and close the dialog box.

.... Creating a New Materials Database and Materials

Using the Create/Edit Materials Dialog Box (p. ), you can create a new materials database, copy

materials to this database, and also create new materials from scratch. The procedure for creating a

new database and add new materials to the database is as follows:

. In the Materials Task Page (p. ), click User-Defined Database....

. In the Open Database Dialog Box (p. ), enter the name of the database that you are creating and click

OK.

. A dialog box will appear asking you confirm the creation of a new file. Click Yes to confirm.

This will open a blank User-Defined Database Materials Dialog Box (p. ) (Figure . : User-Defined

Database Materials Dialog Box: Blank (p. )).

Figure . : User-Defined Database Materials Dialog Box: Blank

. Click New... in the User-Defined Database Materials Dialog Box (p. ).This will open a blank Material

Figure . : Material Properties Dialog Box: Blank

a.

a.

In the Material Properties Dialog Box (p. ), under Types, select the material type.You can select

from fluid, solid, inert-particle, droplet-particle, combusting-particle, and mixture materials.

b. Enter the name and formula (if required) of the material that you are creating in the Name and For-

mula fields.

c.

Depending on the type of material selected in the Types list, properties applicable to that material

type will appear in the Available Properties list. Select the properties that are applicable for the

material that you are defining by clicking on them.

d. Click the

button to move these properties to the Material Properties list on the right and click

Apply.You can use the

button to move the property from the Material Properties list to the

Available Properties list.

. To edit the parameters that define a property, select the property in the Material Properties list and

click Edit....This opens the Edit Property Methods Dialog Box (p. ).

Figure . : Edit Property Methods Dialog Box

a.

The methods that can be used to define the selected property are listed in the Available Properties

list.You can select one or more methods and specify them for the material that you are defining, by

selecting and moving them to the Material Properties list.

b. To modify each of these methods, you can select the method in the Edit Properties drop-down list

and click Edit....This will open the corresponding property dialog box, where you can modify the

parameters used by the property method. Refer to Defining Properties Using Temperature-Dependent

Functions (p. ) to Real Gas Models (p. ) for details of these properties, methods used to define

the properties and the parameters for each method.

c.

Click OK in the Edit Property Methods Dialog Box (p. ).

. Click Apply in the Material Properties Dialog Box (p. ).

. Click Save in the User-Defined Database Materials Dialog Box (p. ) to save the changes to the new

materials database.

Similarly, you can also append new materials and click save to append these materials to the existing

database.

.... Deleting Materials from a Database

To delete a material from a database, click the User-Defined Database button in the Open Database

Dialog Box (p. ). Select the database and click OK in the Open Database Dialog Box (p. ). Select

the Material Type and the materials that you want to delete in the User-Defined Materials list and

click Delete. Click Save to save the database.

Material properties can be defined as functions of temperature. For most properties, you can define a

polynomial, piecewise-linear, or piecewise-polynomial function of temperature.

polynomial:

(.)

piecewise-linear:

(.)

where

and

is the number of segments

piecewise-polynomial:

(.)

In the equations above,

is the property.

Important

If you define a polynomial or piecewise-polynomial function of temperature, the temperature

in the function is always in units of Kelvin or Rankine. If you use Celsius or Kelvin as the

temperature unit, then polynomial coefficient values must be entered in terms of Kelvin. If

you use Fahrenheit or Rankine as the temperature unit, enter the values in terms of Rankine.

Some properties have additional functions available and for some only a subset of these three functions

can be used. See the section on the property in question to determine which temperature-dependent

functions you can use.

... Inputs for Polynomial Functions

... Inputs for Piecewise-Linear Functions

... Inputs for Piecewise-Polynomial Functions

... Checking and Modifying Existing Profiles

To define a polynomial function of temperature for a material property, do the following:

. In the Create/Edit Materials Dialog Box (p. ), choose polynomial in the drop-down list to the right of

the property name (for example, Density).The Polynomial Profile Dialog Box (p. ) (Figure . :The

Polynomial Profile Dialog Box (p. )) will open automatically.

Defining Properties Using Temperature-Dependent Functions

Figure . : The Polynomial Profile Dialog Box

Since this is a modal dialog box, the solver will not allow you to do anything else until you perform

the following steps.

a.

Specify the number of Coefficients up to  coefficients are available.The number of coefficients

defines the order of the polynomial.The default of  defines a polynomial of order .The property

will be constant and equal to the single coefficient

. An input of  defines a polynomial of order

and the property will vary linearly with temperature and so on.

b. Define the coefficients. Coefficients , , ,... correspond to

,

,

,

,

,... in Equation . (p. ).The

dialog box in Figure . :The Polynomial Profile Dialog Box (p. ) shows the inputs for the following

function:

(.)

Important

To ensure the robustness of simulations when using polynomials to specify material property,

set the solution limits so that the values returned by the polynomial expression are physically

valid. For example, when the density of a material is specified as a function of temperature

using a polynomial expression, set the proper limits on the temperature range so that the

density is always non-negative. For more information on setting solution limits see Setting

Solution Limits (p. ).

Also, note the restriction on the units for temperature, as described in the previous section.

To define a piecewise-linear function of temperature for a material property, do the following:

. In the Create/Edit Materials Dialog Box (p. ), choose piecewise-linear in the drop-down list to the right

of the property name (for example, Viscosity).The Piecewise-Linear Profile Dialog Box (p. ) (Fig-

ure . :The Piecewise-Linear Profile Dialog Box (p. )) will open automatically.

Figure . : The Piecewise-Linear Profile Dialog Box

Since this is a modal dialog box, the solver will not allow you to do anything else until you perform the

following steps.

a.

Set the number of Points defining the piecewise distribution.

b. Under Data Points, enter the data pairs for each point. First enter the independent and dependent

a.

variable values for Point , then increase the Point number and enter the appropriate values for each

additional pair of variables.The pairs of points must be supplied in the order of increasing value of

temperature.The solver will not sort them for you. A maximum of  piecewise points can be defined

for each property.The dialog box in Figure . :The Piecewise-Linear Profile Dialog Box (p. ) shows

the final inputs for the profile depicted in Figure . : Piecewise-Linear Definition of Viscosity as a

Function of Temperature (p. ).

Important

If the temperature exceeds the maximum Temperature (

) you have specified

for the profile, ANSYS Fluent will use the Value corresponding to

. If the temper-

ature falls below the minimum Temperature (

) specified for your profile, ANSYS

Fluent will use the Value corresponding to

.

Figure . : Piecewise-Linear Definition of Viscosity as a Function of Temperature

To define a piecewise-polynomial function of temperature for a material property, follow these steps:

. In the Create/Edit Materials Dialog Box (p. ), choose piecewise-polynomial in the drop-down list to

the right of the property name (for example, Cp).The Piecewise-Polynomial Profile Dialog Box (p. )

(Figure . :The Piecewise-Polynomial Profile Dialog Box (p. )) will open automatically. Since this is a

modal dialog box, first perform the following steps.

Figure . : The Piecewise-Polynomial Profile Dialog Box

. Specify the number of Ranges. For the example of Equation . (p. ), two ranges of temperatures are

defined:

(.)

You may define up to three ranges. The ranges must be supplied in the order of increasing value

of temperature. The solver will not sort them for you.

. For the first range (Range = ), specify the Minimum and Maximum temperatures, and the number of

Coefficients. (Up to eight coefficients are available.) The number of coefficients defines the order of the

polynomial.The default of  defines a polynomial of order .The property will be constant and equal to

the single coefficient

. An input of  defines a polynomial of order .The property will vary linearly with

temperature and so on.

. Define the coefficients. Coefficients , , ,... correspond to

,

,

,... in Equation . (p. ).The dialog

box in Figure . :The Piecewise-Polynomial Profile Dialog Box (p. ) shows the inputs for the first range

of Equation . (p. ).

. Increase the value of Range and enter the Minimum and Maximum temperatures, number of Coefficients,

and the Coefficients (

,

,

,...) for the next range. Repeat if there is a third range.

If you want to check or change the coefficients, data pairs, or ranges for a previously-defined profile,

click the Edit... button to the right of the property name. The appropriate dialog box will open, and

you can check or modify the inputs as desired.

Important

In the Fluent Database Materials Dialog Box (p. ), you cannot edit the profiles, but you

can examine them by clicking on the View... button (instead of the Edit... button.)

.. Density

Important

.. Density

ANSYS Fluent provides several options for definition of the fluid density:

constant density

temperature and/or composition-dependent density

pressure-dependent density

Each of these input options and the governing physical models are explained in the following sections.

In all cases, you will define the Density in the Create/Edit Materials Dialog Box (p. ).

Setup →

Materials

Note

For transient, variable-density flows that use the pressure-based solver, you may reach con-

vergence faster if you specify that the model equations are solved in an optimal order. For

details, see Equation Order (p. ).

... Defining Density for Various Flow Regimes

... Input of Constant Density

... Inputs for the Boussinesq Approximation

... Compressible Liquid Density Method

... Density as a Profile Function of Temperature

... Incompressible Ideal Gas Law

... Ideal Gas Law for Compressible Flows

... Composition-Dependent Density for Multicomponent Mixtures

The selection of density in ANSYS Fluent is very important. Set the density relationship based on your

flow regime.

For compressible flows, the ideal gas law is the appropriate density relationship.

For incompressible flows, you may choose one of the following methods:

Density

– Constant density, if you do not want density to be a function of temperature.

– The incompressible ideal gas law, when pressure variations are small enough that the flow is fully incom-

Density

pressible but you want to use the ideal gas law to express the relationship between density and temper-

ature (for example, for a natural convection problem).

– Density as a polynomial, piecewise-linear, or piecewise-polynomial function of temperature, when the

density is a function of temperature only, as in a natural convection problem.

– The Boussinesq model, for natural convection problems involving small changes in temperature.

– The compressible liquid density method allows you to model compressible liquids under high pressures.

.... Mixing Density Relationships in Multiple-Zone Models

If your model has multiple fluid zones that use different materials, you should be aware of the following:

For calculations with the pressure-based solver that do not use one of the general multiphase models

(Solution Strategies for Multiphase Modeling (p. )), the compressible ideal gas law cannot be mixed

with any other density methods.This means that if the compressible ideal gas law is used for one material,

it must be used for all materials.

This restriction does not apply to the density-based solvers.

There is only one specified operating pressure and one specified operating temperature.This means that

if you are using the ideal gas law for more than one material, they will share the same operating pressure.

If you are using the Boussinesq model for more than one material, they will share the same operating

If you want to define the density of the fluid as a constant, select constant in the Density drop-down

list under Properties in the Create/Edit Materials Dialog Box (p. ). Enter the value of density for the

material.

For the default fluid (air), the density is . kg/

.

To enable the Boussinesq approximation for density, choose boussinesq from the Density drop-down

list in the Create/Edit Materials Dialog Box (p. ) and specify a constant value for Density. You will

also need to set the Thermal Expansion Coefficient, as well as relevant operating conditions, as de-

scribed in The Boussinesq Model (p. ).

The compressible liquid treatment enables you to model liquid compressibility under high pressure

applications. Fluent models compressible liquids using the Tait equation of state, which establishes a

nonlinear relationship between density and pressure under isothermal conditions.

The compressible liquid treatment also helps in reducing unphysical pressure spikes that appear in

moving and dynamic mesh applications, especially during solid-fluid interactions.

The Tait equation can be represented in terms of pressure and density using the following relationship:

(.)

where,

and  are coefficients that can be determined by assuming that the bulk modulus is a linear

function of pressure. The values of coefficients  and  are based on the reference state values of

pressure, density, and bulk modulus.

The simplified form of the Tait equation can be written as:

(.)

where,

(.)

and

(.)

where,

= Reference liquid pressure (Absolute)

= Reference liquid density (Density at reference pressure,

)

(.)

where,

(.)

and

(.)

where,

)

= Reference bulk modulus (Bulk modulus at reference pressure,

)

= Density exponent

= Liquid pressure (Absolute)

= Liquid density at pressure,

= Bulk modulus at pressure,

The density ratio is limited to the range:

(.)

where,

= Minimum density ratio limit, when

= Maximum density ratio limit, when

The speed of sound, , is calculated as:

(.)

Note

You can postprocess the speed of sound for compressible liquid materials. For multiphase

models, sound-speed postprocessing is available at mixture and/or phase level, depending

on the model selected. Sound-speed postprocessing is also enabled if you describe the

speed of sound for a user-defined density.

Density

.... Compressible Liquid Inputs

Select the compressible-liquid under Density in the Create/Edit Materials panel as seen in

Figure . : Compressible Liquid Materials Setting (p. ).

Figure . : Compressible Liquid Materials Setting

In the Compressible Liquid dialog box you need to specify values for the following settings:

Reference Pressure

Reference Density

Reference Bulk Modulus

Density Exponent

Maximum Density Ratio Limit

Minimum Density Ratio Limit

Figure . : Compressible Liquid Density Settings Panel

Note

ANSYS Fluent automatically fills user input values for certain materials based on open literature.

If data is not available Fluent will fill in values of zero.Therefore, you must verify that suitable

values are entered for your application.

When Fluent automatically fills in values, the default value of the density exponent is set close

to the value for water-liquid.

The value for the density exponent is generally found by calibrating against data for density,

pressure, bulk modulus, and speed of sound. If the value is unknown, it is recommended that

you use a value of , which corresponds to a linear relationship between density and pressure.

You can set the compressible-liquid density method using the following text command:

define → materials → change-create

In the text command interface, set the change Density? option to yes, and set new method

[constant] to compressible-liquid as shown below:

/define/materials> change-create

material-name> water-liquid

material name [water-liquid]

water-liquid is a fluid

change Density? [no] yes

Density

methods: (constant ideal-gas incompressible-ideal-gas real-gas-soave-redlich-kwong real-gas-peng-robinson

real-gas-aungier-redlich-kwong real-gas-redlich-kwong boussinesq piecewise-linear piecewise-polynomial

polynomial compressible-liquid user-defined)

new method [constant] compressible-liquid

Reference Pressure (pascal) []

Reference Density (kg/m3) [.]

Reference Bulk Modulus (pascal) []

Density Exponent [.]

Maximum Density Ratio Limit [.]

Minimum Density Ratio Limit [.]

Density

.... Compressible Liquid Density Method Availability

The compressible liquid density method is available with fluid materials or with components of a

mixture material having the density method set to volume-weighted-mixing-law for both

single and multiphase cases.

This method is not available with the density-based solver.

If you are modeling a problem that involves heat transfer, you can define the density as a function of

temperature. Three types of functions are available:

(.)

(.)

(.)

For one of the these methods, select piecewise-linear, piecewise-polynomial, or polynomial in the

Density drop-down list. You can enter the data pairs (

), ranges and coefficients, or coefficients

that describe these functions using the Create/Edit Materials Dialog Box (p. ), as described in Defining

Properties Using Temperature-Dependent Functions (p. ).

In ANSYS Fluent, if you choose to define the density using the ideal gas law for an incompressible

flow, the solver will compute the density as

(.)

where,

= the universal gas constant

= the molecular weight of the gas

= the operating pressure

In this form, the density depends only on the operating pressure and not on the local relative pressure

field.

.... Density Inputs for the Incompressible Ideal Gas Law

The inputs for the incompressible ideal gas law are as follows:

. Enable the ideal gas law for an incompressible fluid by choosing incompressible-ideal-gas from the

drop-down list to the right of Density in the Create/Edit Materials Dialog Box (p. ).

Specify the incompressible ideal gas law individually for each material that you want to use it for.

See Composition-Dependent Density for Multicomponent Mixtures (p. ) for information on

specifying the incompressible ideal gas law for mixtures.

. Set the operating pressure by defining the Operating Pressure in the Operating Conditions Dialog

Box (p. ).

Setup →

Important

By default, operating pressure is set to  Pa. The input of the operating pressure

is of great importance when you are computing density with the ideal gas law. See

Operating Pressure (p. ) for recommendations on setting appropriate values for the

operating pressure.

. Set the molecular weight of the homogeneous or single-component fluid (if no chemical species transport

equations are to be solved), or the molecular weights of each fluid material (species) in a multicomponent

mixture. For each fluid material, enter the value of the Molecular Weight in the Create/Edit Materials

For compressible flows, the gas law is as following:

(.)

where,

= the local relative (or gauge) pressure predicted by ANSYS Fluent

.... Density Inputs for the Ideal Gas Law for Compressible Flows

The inputs for the ideal gas law are as follows:

. Enable the ideal gas law for a compressible fluid by choosing ideal-gas from the drop-down list to the

right of Density in the Create/Edit Materials Dialog Box (p. ).

Specify the ideal gas law individually for each material that you want to use it for. See Composition-

Dependent Density for Multicomponent Mixtures (p. ) for information on specifying the ideal

gas law for mixtures.

Box (p. ).

Density

Setup →

Box (p. ).

Density

Setup →

Important

The input of the operating pressure is of great importance when you are computing

density with the ideal gas law. Equation . (p. ) notes that the operating pressure

is added to the relative pressure field computed by the solver, yielding the absolute

static pressure. See Operating Pressure (p. ) for recommendations on setting appro-

priate values for the operating pressure. By default, operating pressure is set to

Pa.

If you are solving species transport equations, set properties for the mixture material and for the con-

stituent fluids (species), as described in detail in Defining Properties for the Mixture and Its Constituent

Species (p. ). To define a composition-dependent density for a mixture, do the following:

. Select the density method:

For non-ideal-gas mixtures, select the volume-weighted-mixing-law method for the mixture material

in the drop-down list to the right of Density in the Create/Edit Materials Dialog Box (p. ).

If you are modeling compressible flow, select ideal-gas for the mixture material in the drop-down list to

the right of Density in the Create/Edit Materials Dialog Box (p. ).

If you are modeling incompressible flow using the ideal gas law, select incompressible-ideal-gas for

the mixture material in the Density drop-down list in the Create/Edit Materials Dialog Box (p. ).

If you have a user-defined function that you want to use to model the density, you can choose either

the user-defined method or the user-defined-mixing-law method for the mixture material in the

drop-down list.

The only difference between the user-defined-mixing-law and the user-defined option for spe-

cifying density, viscosity and thermal conductivity of mixture materials, is that with the user-defined-

mixing-law option, the individual properties of the species materials can also be specified. (Note

that only the constant, the polynomial methods and the user-defined methods are available.)

. Click Change/Create.

. If you have selected volume-weighted-mixing-law, define the density for each of the fluid materials that

make up the mixture.You may define constant or compressible-liquid or (if applicable) temperature-de-

pendent densities for the individual species.

. If you selected user-defined-mixing-law, define the density for each of the fluid materials that make up

the mixture.You may define constant, or (if applicable) temperature-dependent densities, or user-defined

densities for the individual species. More information on defining properties with user-defined functions

can be found in the Fluent Customization Manual.

If you are modeling a non-ideal-gas mixture, ANSYS Fluent will compute the mixture density as

(.)

where

is the mass fraction and

(.)

where

is the density of species .

For compressible flows, the gas law has the following form:

(.)

where,

= the mass fraction of species

= the molecular weight of species

(.)

where,

ANSYS Fluent provides several options for definition of the fluid viscosity:

constant viscosity

temperature-dependent and/or composition-dependent viscosity

kinetic theory

non-Newtonian viscosity

user-defined function

Viscosity

Each of these input options and the governing physical models are detailed in this section. (User-defined

functions are described in the Fluent Customization Manual). In all cases, define the Viscosity in the

Create/Edit Materials Dialog Box (p. ).

Setup →

Materials

Viscosities are input as dynamic viscosity ( ) in units of kg/m-s in SI units or

/ft-s in British units.

ANSYS Fluent does not ask for input of the kinematic viscosity ( ).

... Input of Constant Viscosity

...Viscosity as a Function of Temperature

... Defining the Viscosity Using Kinetic Theory

... Composition-Dependent Viscosity for Multicomponent Mixtures

...Viscosity for Non-Newtonian Fluids

If you want to define the viscosity of your fluid as a constant, select constant in the Viscosity drop-

down list in the Create/Edit Materials Dialog Box (p. ), and enter the value of viscosity for the fluid.

For the default fluid (air), the viscosity is

kg/m-s.

If you are modeling a problem that involves heat transfer, you can define the viscosity as a function

of temperature. Five types of functions are available.

(.)

(.)

(.)

Sutherland’s law

power law

Important

The power law described here is different from the non-Newtonian power law described in

Viscosity for Non-Newtonian Fluids (p. ).

For one of the first three, select piecewise-linear, piecewise-polynomial, polynomial in the Viscosity

drop-down list and then enter the data pairs (

), ranges and coefficients, or coefficients that describe

these functions Defining Properties Using Temperature-Dependent Functions (p. ). For Sutherland’s

law or the power law, choose sutherland or power-law respectively in the drop-down list and enter

the parameters.

.... Sutherland Viscosity Law

Sutherland’s viscosity law resulted from a kinetic theory by Sutherland () using an idealized inter-

molecular-force potential. The formula is specified using two or three coefficients.

Sutherland’s law with two coefficients has the form

(.)

where,

= the viscosity in kg/m-s

= the static temperature in K

and

= the coefficients

For air at moderate temperatures and pressures,

kg/m-s-

, and

K.

(.)

where,

and

kg/m-s-

, and

K.

Sutherland’s law with three coefficients has the form

(.)

where,

= reference value in kg/m-s

= reference temperature in K

= an effective temperature in K (Sutherland constant)

kg/m-s,

= . K, and  =

. K.

..... Inputs for Sutherland’s Law

To use Sutherland’s law, choose sutherland in the drop-down list to the right of Viscosity. The

Sutherland Law Dialog Box (p. ) will open, and you can enter the coefficients as follows:

. Select the Two Coefficient Method or the Three Coefficient Method.

Important

Use SI units if you choose the two-coefficient method.

. For the Two Coefficient Method, set C1 and C2. For the Three Coefficient Method, set the Reference

Viscosity

, the Reference Temperature

, and the Effective Temperature

.

Viscosity

.... Power-Law Viscosity Law

Another common approximation for the viscosity of dilute gases is the power-law form. For dilute

gases at moderate temperatures, this form is considered to be slightly less accurate than Sutherland’s

law.

A power-law viscosity law with two coefficients has the form

(.)

where,

= a dimensional coefficient

, and

.

A power-law viscosity law with three coefficients has the form

(.)

where,

= a reference value in K

= a reference value in kg/m-s

kg/m-s,

K, and

.

Important

kg/m-s,

K, and

.

Important

The non-Newtonian power law for viscosity is described in Viscosity for Non-Newtonian

Fluids (p. ).

..... Inputs for the Power Law

To use the power law, choose power-law in the drop-down list to the right of Viscosity. The Power

Law Dialog Box (p. ) will open, and you can enter the coefficients as follows:

Important

Note that you must use SI units if you choose the two-coefficient method.

. For the Two Coefficient Method, set B and the Temperature Exponent

. For the Three Coefficient

Method, set the Reference Viscosity

, and the Temperature Expo-

nent

.

If you are using the ideal gas law (as described in Density (p. )), you have the option to define the

fluid viscosity using kinetic theory as

(.)

where,

is in units of kg/m-s,

is in units of Kelvin

is in units of Angstroms

is the molecular weight

where

(.)

The Lennard-Jones parameters,

and

, are inputs to the kinetic theory calculation that you

supply by selecting kinetic-theory from the drop-down list to the right of Viscosity in the Create/Edit

Materials Dialog Box (p. ). The solver will use these kinetic theory inputs in Equation . (p. ) to

compute the fluid viscosity. See Kinetic Theory Parameters (p. ) for details about these inputs.

If you are modeling a flow that includes more than one chemical species (multicomponent flow), you

have the option to define a composition-dependent viscosity. (Note that you can also define the vis-

cosity of the mixture as a constant value or a function of temperature.)

To define a composition-dependent viscosity for a mixture, follow these steps:

. For the mixture material, choose mass-weighted-mixing-law or, if you are using the ideal gas law for

density, ideal-gas-mixing-law in the drop-down list to the right of Viscosity. If you have a user-defined

function that you want to use to model the viscosity, you can choose either the user-defined method or

the user-defined-mixing-law method for the mixture material in the drop-down list.

. Define the viscosity for each of the fluid materials that make up the mixture.You may define constant or

(if applicable) temperature-dependent viscosities for the individual species.You may also use kinetic

theory for the individual viscosities, or specify a non-Newtonian viscosity, if applicable.

. If you selected user-defined-mixing-law, define the viscosity for each of the fluid materials that make

up the mixture.You may define constant, or (if applicable) temperature-dependent viscosities, or user-

defined viscosities for the individual species. More information on defining properties with user-defined

functions can be found in the Fluent Customization Manual.

Viscosity

Viscosity

If you are using the ideal gas law, the solver will compute the mixture viscosity based on kinetic theory

as

(.)

where

(.)

and

is the mole fraction of species .

For non-ideal gas mixtures, the mixture viscosity is computed based on a simple mass fraction average

of the pure species viscosities:

(.)

For incompressible Newtonian fluids, the shear stress is proportional to the rate-of-deformation tensor

:

(.)

where

is defined by

(.)

and  is the viscosity, which is independent of

.

For some non-Newtonian fluids, the shear stress can similarly be written in terms of a non-Newtonian

viscosity :

(.)

In general,

is a function of all three invariants of the rate-of-deformation tensor

. However, in the

non-Newtonian models available in ANSYS Fluent,

is considered to be a function of the shear rate

only.

is related to the second invariant of

and is defined as

(.)

....Temperature Dependent Viscosity

If the flow is non-isothermal, then the temperature dependence on the viscosity can be included

along with the shear rate dependence. In this case, the total viscosity consists of two parts and is

calculated as

(.)

where H(T) is the temperature dependence, known as the Arrhenius law.

(.)

where  is the ratio of the activation energy to the thermodynamic constant and

is a reference

temperature for which H(T) = .

, which is the temperature shift, is set to  by default, and corres-

ponds to the lowest temperature that is thermodynamically acceptable. Therefore

and

are ab-

solute temperatures. Temperature dependence is only included when the energy equation is enabled.

Set the parameter  to  when you want temperature dependence to be ignored, even when the

energy equation is solved.

ANSYS Fluent provides four options for modeling non-Newtonian flows:

power law

Carreau model for pseudo-plastics

Cross model

Herschel-Bulkley model for Bingham plastics

Important

Note that the models listed above are not available when modeling turbulent flow.

Note that the non-Newtonian power law described below is different from the power law de-

scribed in Power-Law Viscosity Law (p. ).

Non-Newtonian model based on single fluid formulation is available for the mixture model

and it is recommended that this should be attached to the primary phase.

Appropriate values for the input parameters for these models can be found in the literature (for ex-

ample, [] (p. )).

.... Power Law for Non-Newtonian Viscosity

If you choose non-newtonian-power-law in the drop-down list to the right of Viscosity, non-Newto-

nian flow will be modeled according to the following power law for the non-Newtonian viscosity:

(.)

where  and  are input parameters.

is a measure of the average viscosity of the fluid (the consist-

ency index);

is a measure of the deviation of the fluid from Newtonian (the power-law index). The

value of  determines the class of the fluid:

Viscosity

→ Newtonian fluid

→ shear-thickening (dilatant fluids)

→ shear-thinning (pseudo-plastics)

Viscosity

..... Inputs for the Non-Newtonian Power Law

To use the non-Newtonian power law, choose non-newtonian-power-law in the drop-down list to

the right of Viscosity. The Non-Newtonian Power Law Dialog Box (p. ) will open, and you can

choose between Shear Rate Dependent and Shear Rate and Temperature Dependent. Enter the

Consistency Index

, Power-Law Index

, Minimum and Maximum Viscosity Limit, Reference

, and Activation Energy/R,

, which is the ratio of the activation energy to the

thermodynamic constant.

....The Carreau Model for Pseudo-Plastics

The power law model described in Equation . (p. ) results in a fluid viscosity that varies with

shear rate. For

,

, and for

,

, where

and

are, respectively, the upper and

lower limiting values of the fluid viscosity.

The Carreau model attempts to describe a wide range of fluids by the establishment of a curve-fit to

piece together functions for both Newtonian and shear-thinning (

) non-Newtonian laws. In the

Carreau model, the viscosity is

(.)

and the parameters ,

,

,

, and

are dependent upon the fluid.

is the time constant,

is

the power-law index (as described above for the non-Newtonian power law),

and

are, respectively,

the zero- and infinite-shear viscosities,

is the reference temperature, and  is the ratio of the ac-

tivation energy to thermodynamic constant. Figure . : Variation of Viscosity with Shear Rate According

to the Carreau Model (p. ) shows how viscosity is limited by

and

at low and high shear rates.

Figure . : Variation of Viscosity with Shear Rate According to the Carreau Model

..... Inputs for the Carreau Model

and

To use the Carreau model, choose carreau in the drop-down list to the right of Viscosity. The Carreau

Model Dialog Box (p. ) will open, and you can choose between Shear Rate Dependent and Shear

Rate and Temperature Dependent. Enter the Time Constant

, Reference

, Zero Shear Viscosity

, Infinite Shear Viscosity

, and Activation Energy/R

.

Figure . : The Carreau Model Dialog Box

.... Cross Model

The Cross model for viscosity is:

(.)

where,

= zero-shear-rate viscosity

= natural time (that is, inverse of the shear rate at which the fluid changes from

Newtonian to power-law behavior)

= power-law index

The Cross model is commonly used to describe the low-shear-rate behavior of the viscosity.

..... Inputs for the Cross Model

To use the Cross model, choose cross in the drop-down list to the right of Viscosity. The Cross

Rate and Temperature Dependent. Enter the Zero Shear Viscosity

, Time Constant

, Power-

Law Index

, Reference Temperature

, which is the ratio of the

activation energy to the thermodynamic constant.

Viscosity

.... Herschel-Bulkley Model for Bingham Plastics

The power law model described above is valid for fluids for which the shear stress is zero when the

strain rate is zero. Bingham plastics are characterized by a nonzero shear stress when the strain rate

is zero.

(.)

where

is the yield stress:

For

, the material remains rigid.

For

, the material flows as a power-law fluid.

is zero.

(.)

where

For

For

The Herschel-Bulkley model combines the effects of Bingham and power-law behavior in a fluid. For

low strain rates (

), the “rigid” material acts like a very viscous fluid with viscosity

. As the

strain rate increases and the yield stress threshold,

, is passed, the fluid behavior is described by a

power law.

For

(.)

For

(.)

where  is the consistency index, and  is the power-law index.

Figure . : Variation of Shear Stress with Shear Rate According to the Herschel-Bulkley Model (p. )

shows how shear stress ( ) varies with shear rate ( ) for the Herschel-Bulkley model.

Figure . : Variation of Shear Stress with Shear Rate According to the Herschel-Bulkley Model

If you choose the Herschel-Bulkley model for Bingham plastics, Equation . (p. ) will be used to

determine the fluid viscosity.

The Herschel-Bulkley model is commonly used to describe materials such as concrete, mud, dough,

and toothpaste, for which a constant viscosity after a critical shear stress is a reasonable assumption.

In addition to the transition behavior between a flow and no-flow regime, the Herschel-Bulkley

model can also exhibit a shear-thinning or shear-thickening behavior depending on the value of .

..... Inputs for the Herschel-Bulkley Model

To use the Herschel-Bulkley model, choose herschel-bulkley in the drop-down list to the right of

Viscosity. The Herschel-Bulkley Dialog Box (p. ) will open, and you can choose between Shear

Rate Dependent and Shear Rate and Temperature Dependent. Enter the Consistency Index

,

Power-Law Index

, Yield Stress Threshold

, Critical Shear Rate

,

, and the ratio of the activation energy to thermodynamic constant , Activation Energy/R.

The thermal conductivity must be defined when heat transfer is active. You must define thermal con-

ductivity when you are modeling energy and viscous flow.

ANSYS Fluent provides several options for definition of the thermal conductivity:

constant thermal conductivity

temperature- and/or composition-dependent thermal conductivity

anisotropic (anisotropic, biaxial, orthotropic, cylindrical orthotropic, principal axes and principal values, user-

defined anisotropic) (for solid materials only)

user-defined

Each of these input options and the governing physical models are detailed in this section. User-defined

functions (UDFs) are described in the Fluent Customization Manual.

In all cases, you will define the Thermal Conductivity in the Create/Edit Materials Dialog Box (p. )

(Figure . : The Create/Edit Materials Dialog Box (p. )).

Setup →

Materials → Create/Edit...

Figure . : The Create/Edit Materials Dialog Box

Thermal conductivity is defined in units of W/m-K in SI units or BTU/hr-ft-°R in British units.

... Constant Thermal Conductivity

...Thermal Conductivity as a Function of Temperature

...Thermal Conductivity Using Kinetic Theory

... Composition-Dependent Thermal Conductivity for Multicomponent Mixtures

... Anisotropic Thermal Conductivity for Solids

If you want to define the thermal conductivity as a constant, check that constant is selected in the

drop-down list to the right of Thermal Conductivity in the Create/Edit Materials Dialog Box (p. )

(Figure . : The Create/Edit Materials Dialog Box (p. )), and enter the value of thermal conductivity

for the material.

For the default fluid (air), the thermal conductivity is . W/m-K.

You can also choose to define the thermal conductivity as a function of temperature. Three types of

functions are available:

(.)

(.)

(.)

You can input the data pairs (

), ranges and coefficients

and

, or coefficients

that describe

these functions using the Create/Edit Materials Dialog Box (p. ), as described in Defining Properties

Using Temperature-Dependent Functions (p. ).

thermal conductivity using kinetic theory as

(.)

where  is the universal gas constant,

is the molecular weight,

is the material’s specified or

computed viscosity, and

is the material’s specified or computed specific heat capacity.

To enable the use of this equation for calculating thermal conductivity, select kinetic-theory from the

drop-down list to the right of Thermal Conductivity in the Create/Edit Materials Dialog Box (p. ).

The solver will use Equation . (p. ) to compute the thermal conductivity.

... Composition-Dependent Thermal Conductivity for Multicomponent

Mixtures

have the option to define a composition-dependent thermal conductivity. (Note that you can also

define the thermal conductivity of the mixture as a constant value or a function of temperature, or

using kinetic theory.)

To define a composition-dependent thermal conductivity for a mixture, follow these steps:

. For the mixture material, choose mass-weighted-mixing-law or, if you are using the ideal gas law, ideal-

gas-mixing-law in the drop-down list to the right of Thermal Conductivity. If you have a user-defined

function that you want to use to model the thermal conductivity, you can choose either the user-defined

method or the user-defined-mixing-law method for the mixture material in the drop-down list.

mixing-law option, the individual properties of the species materials can also be specified. Note

that only the constant, the polynomial methods and the user-defined methods are available.

Important

If you use ideal-gas-mixing-law for the thermal conductivity of a mixture, you must

use ideal-gas-mixing-law or mass-weighted-mixing-law for viscosity, because these

two viscosity specification methods are the only ones that allow specification of the

component viscosities, which are used in the ideal gas law for thermal conductivity

(Equation . (p. )).

. Define the thermal conductivity for each of the fluid materials that make up the mixture.You may define

constant or (if applicable) temperature-dependent thermal conductivities for the individual species.You

may also use kinetic theory for the individual thermal conductivities, if applicable.

. If you selected user-defined-mixing-law, define the thermal conductivity for each of the fluid materials

that make up the mixture.You may define constant, or (if applicable) temperature-dependent thermal

conductivities, or user-defined thermal conductivities for the individual species. More information about

defining properties with user-defined functions can be found in the Fluent Customization Manual.

If you are using the ideal gas law, the solver will compute the mixture thermal conductivity based on

kinetic theory as

(.)

where

(.)

and

For non-ideal gases, the mixture thermal conductivity is computed based on a simple mass fraction

average of the pure species conductivities:

(.)

The anisotropic conductivity option in ANSYS Fluent solves the conduction equation in solid zones

and shells with the thermal conductivity specified as a matrix. The heat flux vector is written as

(.)

The following options are available for defining anisotropic thermal conductivity in ANSYS Fluent.

These are discussed below.

anisotropic

biaxial (available for shells only)

(.)

orthotropic

cylindrical orthotropic

principal axes and principal values

user-defined anisotropic

Note

When postprocessing solid material properties, the Thermal Conductivity will be displayed

as zero if an anisotropic thermal conductivity model is being used for a solid material.

Important

The anisotropic conductivity options are available only with the pressure-based solver; you

cannot use them with the density-based solvers.

.... Anisotropic Thermal Conductivity

For anisotropic diffusion, the thermal conductivity matrix (Equation . (p. )) is specified as

(.)

where  is the conductivity and

is a matrix (   for two dimensions and    for three-dimen-

sional problems). Note that

can be a non-symmetric matrix.

To define anisotropic thermal conductivity for a solid material, select anisotropic for Thermal Con-

ductivity in the Create/Edit Materials Dialog Box (p. ) (Figure . : The Create/Edit Materials Dialog

Box (p. )). Note the following:

If the principal axes of your anisotropic material are not aligned with the global coordinate system of your

simulation, it may be easier for you to use one of the following options: if the axes are orthogonal, you

can use the orthotropic option, as described in Orthotropic Thermal Conductivity (p. ); if the axes are

not orthogonal, you can use the principal-axes-values option, as described in Principal Axes and Principal

Values (p. ). If you use the anisotropic option with unaligned axes, it is your responsibility to transform

the thermal conductivity properties into the

tensor aligned with the global coordinate system.

The anisotropic option is appropriate when the components of the

matrix are constants and do not

vary independently; if this is not the case, you can use a UDF to define the matrix and select user-defined-

anisotropic-k, as described in User-Defined Anisotropic Thermal Conductivity (p. ).

Selecting anisotropic will open the Anisotropic Conductivity Dialog Box (p. ) (Figure . : The An-

isotropic Conductivity Dialog Box (p. )).

Figure . : The Anisotropic Conductivity Dialog Box

In the Anisotropic Conductivity Dialog Box (p. ), enter the Matrix Components of matrix

and

then select the Conductivity (  in Equation . (p. )) to be a constant, polynomial function of

temperature (polynomial, piecewise-linear, piecewise-polynomial), or user-defined function. See

Constant Thermal Conductivity (p. ) and Thermal Conductivity as a Function of Temperature (p. )

for details on constants and thermal polynomial functions.

When you select the user-defined option, the User-Defined Functions Dialog Box (p. ) will open,

allowing you to hook a DEFINE_PROPERTY UDF only if you have previously loaded a compiled UDF

library or interpreted the UDF. Otherwise, you will get an error message. Details about user-defined

.... Biaxial Thermal Conductivity

Biaxial thermal conductivity is applicable only for solid materials used for the wall shell conduction

model. To define a biaxial thermal conductivity, select biaxial in the drop-down list for Thermal

Conductivity in the Create/Edit Materials Dialog Box (p. ). This opens the Biaxial Conductivity

Dialog Box (p. ) (Figure . : The Biaxial Conductivity Dialog Box (p. )).

Figure . : The Biaxial Conductivity Dialog Box

In the Biaxial Conductivity Dialog Box (p. ), both the conductivity normal to the surface of the shell

(Transverse Conductivity) and the conductivity parallel to the surface of the shell (Planar Conduct-

ivity) can be defined as constant, polynomial, piecewise-linear, or piecewise-polynomial. See

for details on these parameters. Note that the Planar Conductivity is isotropic. See Figure . : The

Shell Conduction Manager Dialog Box (p. ).

.... Orthotropic Thermal Conductivity

When the orthotropic thermal conductivity is used, the thermal conductivities

in the

principal directions

are specified. The conductivity matrix is then computed as

(.)

To define an orthotropic thermal conductivity in solids, select orthotropic in the drop-down list for

Thermal Conductivity in the Create/Edit Materials Dialog Box (p. ). This opens the Orthotropic

Conductivity Dialog Box (p. ) (Figure . : The Orthotropic Conductivity Dialog Box (p. )).

Figure . : The Orthotropic Conductivity Dialog Box

Since the directions

are mutually orthogonal, only the first two need to be specified for

three-dimensional problems.

is defined using X, Y, Z under Direction  Components, and

is

defined using X, Y, Z under Direction  Components. You can define Conductivity

, Conduct-

ivity

, and Conductivity

is

, Conduct-

ivity

as constant, polynomial, piecewise-linear, piecewise-poly-

nomial functions of temperature, or user-defined. See Constant Thermal Conductivity (p. ) and

Thermal Conductivity as a Function of Temperature (p. ) for details on constant and temperature

profile functions.

library or interpreted the UDF. Otherwise, you will get an error message. More information about

user-defined functions can be found in the Fluent Customization Manual.

Important

For two-dimensional problems, only the functions

and the unit vector

need

to be specified.

.... Cylindrical Orthotropic Thermal Conductivity

The orthotropic conductivity of solids can be specified in cylindrical coordinates. To define the ortho-

tropic thermal conductivity in cylindrical coordinates, select cyl-orthotropic in the drop-down list for

Thermal Conductivity in the Create/Edit Materials Dialog Box (p. ). This opens the Cylindrical Or-

thotropic Conductivity Dialog Box (p. ) (Figure . : The Cylindrical Orthotropic Conductivity Dialog

Box (p. )).

Figure . : The Cylindrical Orthotropic Conductivity Dialog Box

In three-dimensional cases, the origin and the direction of the cylindrical coordinate system must be

specified along with the radial, tangential, and axial direction conductivities. In two-dimensional cases,

the origin of the cylindrical coordinate system must be specified along with the radial and tangential

direction conductivities. Note that in two-dimensional cases, the direction is always along the +Z axis.

ANSYS Fluent will automatically compute the anisotropic conductivity matrix at each cell from this

input. The calculation is based on the location of the cell in the cylindrical coordinate system specified.

You can define the Radial Conductivity, Tangential Conductivity, and Axial Conductivity as con-

stant, polynomial, piecewise-linear, piecewise-polynomial, or as user-defined functions of temper-

ature. See Constant Thermal Conductivity (p. ) and Thermal Conductivity as a Function of Temper-

ature (p. ) for details on constant and thermal profile functions.

Important

For conductivity calculations near the wall, the cell next to the wall is chosen for computing

the conductivity matrix instead of the wall itself.

.... Principal Axes and Principal Values

When the principal axes of your anisotropic material are not aligned with the global coordinate system

of the simulation, you can define the thermal conductivity using the components of these axes (

,

, and for 3D problems,

) and the associated principle values (

,

).

,

,

).

The axes take the following form:

(.)

Note that while the axes must be linearly independent vectors, they do not have to be unit vectors

or orthogonal.

An example of principal axes that are not aligned with the global coordinate system is shown in

Figure . : Unaligned Principal Axes (p. ).

Figure . : Unaligned Principal Axes

Representing the thermal conductivity matrix (

in Equation . (p. )) in matrix notation (

),

the following equation is used by ANSYS Fluent to transform the principal axes and principal values

into the correct tensor form:

(.)

The matrices in the previous equation are defined as follows:

(.)

(.)

where  is the conductivity.

To use principal axes and principal values to define the anisotropic thermal conductivity for your

solid material, select principal-axes-values for Thermal Conductivity in the Create/Edit Materials

Dialog Box (p. ) (Figure . : The Create/Edit Materials Dialog Box (p. )). This will open the Aniso-

tropic Conduction - Principal Components Dialog Box (p. ) (Figure . : The Anisotropic Conductivity

Principal Components Dialog Box (p. )).

Figure . : The Anisotropic Conductivity - Principal Components Dialog Box

In the Principal Axes group box of the Anisotropic Conduction - Principal Components Dialog

Box (p. ), enter the i, j, and k components for each of the n1, n2, and n3 vectors (Equa-

tion . (p. )) that define the principal axes of your material in the global coordinate system; note

that these must be linearly independent vectors. Then in the Principal Values group box, enter the

K1, K2, and K3 values that define the magnitudes of the principal values along the associated prin-

cipal axes. Finally, make a selection from the Conductivity drop-down menu to specify  (in Equa-

tion . (p. )) as a constant, polynomial function of temperature (polynomial, piecewise-linear,

piecewise-polynomial), or user-defined function, and then define it using the number-entry box

that becomes available or the dialog box that opens. See Constant Thermal Conductivity (p. ) and

Thermal Conductivity as a Function of Temperature (p. ) for details on constants and thermal

.... User-Defined Anisotropic Thermal Conductivity

You have the option of modeling anisotropic conduction for domains where the components of the

thermal conductivity matrix (

in Equation . (p. )) are not constants and vary independently,

perhaps as a function of space or because the domain has many anisotropic materials stitched together

to form a composite. To use this option, you must first define the conductivity matrix using a UDF,

as described in DEFINE_ANISOTROPIC_CONDUCTIVITY in the Fluent Customization Manual.

After you have interpreted or compiled the DEFINE_ANISOTROPIC_CONDUCTIVITY UDF, you

must then select user-defined-anisotropic-k for Thermal Conductivity in the Create/Edit Materials

Dialog Box (p. ). This will open the User-Defined Functions Dialog Box (p. ), which you can use

to hook the UDF.

There are two types of UDS diffusivity that you can specify in ANSYS Fluent: isotropic and anisotropic.

Diffusion is isotropic when it is the same in all directions. Isotropic diffusion coefficients can be specified

in two ways: either as a single user-defined that applies to all UDS transport equations defined for

your model; or on a per-scalar basis as constants, polynomial functions of temperature, or user-defined

Diffusion is anisotropic when the diffusion coefficients are different in different directions. Anisotropic

diffusion can be specified by a tensor diffusion coefficient matrix  (Equation . (p. )) for each UDS

(in both fluid and solid zones) in four different ways: general anisotropic, orthotropic, cyl-orthotropic,

and user-defined-anisotropic. All UDS diffusivity parameters are set from the Create/Edit Materials

Dialog Box (p. ) and are discussed below. Note that details about how to define and use UDFs in

UDS transport equations is discussed in the Fluent Customization Manual.

The second-order diffusion term in the most general form is

(.)

where  is a    tensor in 3D.

... Isotropic Diffusion

... Anisotropic Diffusion

(.)

... User-Defined Anisotropic Diffusivity

For isotropic diffusion,

in Equation . (p. ) is equal to a scalar  times the identity matrix and

the equation reduces to

(.)

You can specify isotropic diffusivity as a single user-defined function that applies to all UDS transport

equations. For this case, choose user-defined from the drop-down list for UDS Diffusivity in the

Setup →

Materials

If you have previously loaded a compiled UDF library or have interpreted the UDF, then the User-

Defined Functions Dialog Box (p. ) will open, allowing you to hook the DEFINE_DIFFUSIVITY

UDF to ANSYS Fluent. If no functions have been loaded, you will get an error message. More information

about user-defined functions can be found in the Fluent Customization Manual.

Isotropic diffusion coefficients can also be defined on a per-scalar basis by selecting defined-per-uds

from the drop-down list for UDS Diffusivity in the Create/Edit Materials Dialog Box (p. ). This will

open the UDS Diffusion Coefficients Dialog Box (p. ) (Figure . : The UDS Diffusion Coefficients

User-Defined Scalar (UDS) Diffusivity

Figure . : The UDS Diffusion Coefficients Dialog Box

In the UDS Diffusion Coefficients Dialog Box (p. ), select a scalar equation (for example, uds-) and

then choose a constant, polynomial, or user-defined function from the Coefficient drop-down list.

For the default fluid (air), the constant diffusion coefficient is  kg/m-s. If you choose polynomial, the

Polynomial Profile Dialog Box (p. ) will open and you can specify your coefficients as a function of

temperature. See Inputs for Polynomial Functions (p. ) for details.

allowing you to hook a DEFINE_DIFFUSIVITY UDF only if you have previously loaded a compiled

UDF library or interpreted a UDF. Otherwise, you will get an error message. More information about

You can specify anisotropic diffusion coefficients in both fluid and solid zones by defining the tensor

diffusion coefficient matrix  (Equation . (p. )) on a per-scalar basis. You can use anisotropic

diffusivity for UDS scalar transport equations to model species transport equations in porous media

and in solids where species diffusion shows anisotropic behavior.

Important

Note that the anisotropic diffusion options discussed in the following sections are available with

the pressure-based solver and the density-based solvers.

UDS diffusion coefficients can be postprocessed only in those cells that have isotropic diffusivity.

In all other cells, the diffusion coefficient will be zero.

In all cases, you enable anisotropic diffusion by selecting defined-per-uds under UDS Diffusivity in

the Create/Edit Materials Dialog Box (p. ). This will open the UDS Diffusion Coefficients Dialog

Box (p. ) (Figure . : The UDS Diffusion Coefficients Dialog Box (p. )).

Setup →

Materials

Setup →

Materials

then choose one of the following methods under Coefficient to specify the anisotropic diffusion

coefficient. These methods are described in detail below.

.... Anisotropic Diffusivity

For anisotropic diffusivity, you can specify  in Equation . (p. ) in the form

where

is a

constant

matrix in 3D and  is a scalar multiplier.

The diffusion coefficient matrix is specified as

(.)

where  is the diffusivity and

is a matrix (   for two dimensions and    for three-dimensional

problems). Note that

To specify anisotropic diffusion coefficients, first select a scalar equation (for example, uds-) from

the User-Defined Scalar Diffusion list in the UDS Diffusion Coefficients Dialog Box (p. ) (Fig-

ure . : The UDS Diffusion Coefficients Dialog Box (p. )). Then choose anisotropic in the drop-

down list under Coefficient. This will open the Anisotropic UDS Diffusivity dialog box (Figure . : The

Anisotropic UDS Diffusivity Dialog Box (p. )).

Figure . : The Anisotropic UDS Diffusivity Dialog Box

In the Anisotropic UDS Diffusivity dialog box, enter the Matrix Components and then select the

Diffusivity to be a constant, polynomial function of temperature (polynomial, piecewise-linear,

piecewise-polynomial), or user-defined. See Inputs for Polynomial Functions (p. ), Inputs for

Piecewise-Linear Functions (p. ), and Inputs for Piecewise-Polynomial Functions (p. ) for details

on polynomial temperature functions.

.... Orthotropic Diffusivity

For orthotropic diffusivity, you can specify  in Equation . (p. ) through ’principal’ direction

vectors and diffusion coefficients along these directions. ANSYS Fluent, in turn, computes  from

parameters that you supply. The principal directions are the same everywhere, but each of he direc-

tional diffusion coefficients can be specified as a constant, polynomial function of temperature, or

through user-defined functions.

When orthotropic diffusivity is used, the diffusion coefficients

in the principal directions

are specified. The diffusivity matrix is then computed as

(.)

Important

need

To specify orthotropic diffusion coefficients, first select a scalar equation (for example, uds-) from

ure . : The UDS Diffusion Coefficients Dialog Box (p. )). Then choose orthotropic in the drop-

down list under Coefficient. This will open the Orthotropic UDS Diffusivity dialog box (Fig-

ure . : The Orthotropic UDS Diffusivity Dialog Box (p. )).

Figure . : The Orthotropic UDS Diffusivity Dialog Box

is defined using X,Y,Z under Direction  Components, and

is

defined using X,Y,Z under Direction  Components. You can define Diffusivity

, Diffusivity

, and Diffusivity

as constant, polynomial, piecewise-linear, piecewise-polynomial

functions of temperature, or user-defined. See Inputs for Polynomial Functions (p. ), Inputs for

UDF library or interpreted a UDF. If no functions have been loaded, you will get an error message.

More information about user-defined functions can be found in the Fluent Customization Manual.

.... Cylindrical Orthotropic Diffusivity

Orthotropic UDS diffusivity can also be specified on a per-scalar basis in cylindrical coordinates. This

method is similar to orthotropic UDS diffusivity, except that the principal directions are specified as

radial, tangential, and axial.

To specify cylindrical orthotropic diffusion coefficients, first select a scalar equation (for example, uds-

) from the User-Defined Scalar Diffusion list in the UDS Diffusion Coefficients Dialog Box (p. )

(Figure . : The UDS Diffusion Coefficients Dialog Box (p. )). Then choose cyl-orthotropic in the

drop-down list under Coefficient. This will open the Cylindrical Orthotropic UDS Diffusivity dialog

box (Figure . : The Cylindrical Orthotropic UDS Diffusivity Dialog Box (p. )).

Figure . : The Cylindrical Orthotropic UDS Diffusivity Dialog Box

direction conductivities. Note that in two-dimensional cases, the direction is always along the +z axis.

ANSYS Fluent will automatically compute the anisotropic diffusivity matrix at each cell from this input.

The calculation is based on the location of the cell in the cylindrical coordinate system specified.

You can define the Radial Diffusivity, Tangential Diffusivity, and Axial Diffusivity as constant,

polynomial, piecewise-linear, piecewise-polynomial, or as user-defined functions of temperature,

using the drop-down list below each of the diffusivities. See Inputs for Polynomial Functions (p. ),

Inputs for Piecewise-Linear Functions (p. ), and Inputs for Piecewise-Polynomial Functions (p. )

for details on polynomial temperature functions.

You can specify  in Equation . (p. ) on a per-scalar basis, directly, through user-defined functions

(UDFs).

To specify a UDF for anisotropic diffusivity on a per-scalar basis, first select a scalar equation (for example,

uds-) from the User-Defined Scalar Diffusion list in the UDS Diffusion Coefficients Dialog Box (p. )

(Figure . : The UDS Diffusion Coefficients Dialog Box (p. )).

Then choose user-defined-anisotropic in the drop-down list under Coefficient. The User-Defined

Functions Dialog Box (p. ) will open, allowing you to hook a DEFINE_ANISOTROPIC_DIFFUSIVITY

UDF only if you have previously loaded a compiled UDF library or interpreted a UDF. Otherwise, you

will get an error message. More information about user-defined functions can be found in the Fluent

The specific heat capacity must be defined when the energy equation is active. ANSYS Fluent provides

several options for definition of the heat capacity:

constant heat capacity

temperature- and/or composition-dependent heat capacity

Each of these input options and the governing physical models are detailed in this section. In all cases,

you will define the Cp in the Create/Edit Materials Dialog Box (p. ).

Setup →

Setup →

Materials

Specific heat capacity is input in units of J/kg-K in SI units or BTU/lbm-°R in British units.

Important

For combustion applications, a temperature-dependent specific heat is recommended.

... Input of Constant Specific Heat Capacity

... Specific Heat Capacity as a Function of Temperature

... Defining Specific Heat Capacity Using Kinetic Theory

... Specific Heat Capacity as a Function of Composition

If you want to define the heat capacity as a constant, check that constant is selected in the drop-down

list to the right of Cp in the Create/Edit Materials Dialog Box (p. ), and enter the value of heat capacity.

The specific heat for the default fluid (air) is . J/kg-K.

You can also choose to define the specific heat capacity as a function of temperature. Three types of

(.)

(.)

(.)

and

specific heat capacity using kinetic theory as

(.)

where

(.)

where

is the number of modes of energy storage (degrees of freedom) for the gas species  that

you can input by selecting kinetic-theory from the drop-down list to the right of Cp in the Create/Edit

Materials Dialog Box (p. ). The solver will use your kinetic theory inputs in Equation . (p. ) to

compute the specific heat capacity. See Kinetic Theory Parameters (p. ) for details about kinetic

theory inputs.

have the option to define a composition-dependent specific heat capacity. You can also define the

heat capacity of the mixture as a constant value or a function of temperature, or using kinetic theory.

To define a composition-dependent specific heat capacity for a mixture, follow these steps:

. For the mixture material, choose mixing-law in the drop-down list to the right of Cp.

. Define the specific heat capacity for each of the fluid materials that make up the mixture.You may define

constant or (if applicable) temperature-dependent heat capacities for the individual species.You may

also use kinetic theory for the individual heat capacities, if applicable.

The solver will compute the mixture’s specific heat capacity as a mass fraction average of the pure

species heat capacities:

(.)

When you have activated one of the radiation models (except for the surface-to-surface model, which

requires no additional properties), there will be additional properties for you to set in the Create/Edit

Materials Dialog Box (p. ):

For the P- model, you must set the radiation Absorption Coefficient and Scattering Coefficient (  and

in Equation . in the Theory Guide).

For the Rosseland model, set the Absorption Coefficient and Scattering Coefficient (  and

in Equa-

tion . in the Theory Guide).

For the DTRM, only the Absorption Coefficient is required (  in Equation . in the Theory Guide).

Radiation Properties

For the DO model, set the Absorption Coefficient and the Scattering Coefficient (  and

in Equation .

in the Theory Guide). In addition, if you are modeling semi-transparent media, specify the Refractive Index

(

or

in Equation . in the Theory Guide).With the DO model, you can specify radiation properties for

solid materials, to be used when semi-transparent media are modeled.

For the MC model, set the Absorption Coefficient and the Scattering Coefficient (  and

(

or

in Equation . in the Theory Guide).With the MC model, you can specify radiation properties for

... Absorption Coefficient

... Scattering Coefficient

... Refractive Index

... Reporting the Radiation Properties

To define the absorption coefficient, you can specify a constant value, a temperature-dependent

function (see Defining Properties Using Temperature-Dependent Functions (p. )), a composition-

dependent function, or a user-defined function. The absorbing and emitting parts of the radiative

transfer equation (RTE), Equation . in the Theory Guide, is a function of the absorption coefficient.

The absorbing or emitting effects depend on the chosen radiation model. If there are only absorption

effects, then Lambert’s Law of absorption applies

(.)

where  is the radiation intensity,

is the absorption coefficient, and  is the distance through the

material.

If you are modeling non-gray radiation with the P-, DO, or MC radiation models, you also have the

option to specify a constant absorption coefficient in each of the gray bands. The absorption coefficient

is requested in units of /length. Along with the scattering coefficient, it describes the change in radi-

ation intensity per unit length along the path through the fluid medium. Absorption coefficients can

be computed using tables of emissivity for

and

O, which are generally available in textbooks

on radiation heat transfer.

.... Inputs for a Constant Absorption Coefficient

To define a constant absorption coefficient, simply enter the value in the field next to Absorption

Coefficient in the Create/Edit Materials Dialog Box (p. ). Select constant in the drop-down list first

if it is not already selected.

.... Inputs for a Composition-Dependent Absorption Coefficient

ANSYS Fluent also allows you to input a composition-dependent absorption coefficient, where the

local value of  is a function of the local mass fractions of water vapor and carbon dioxide. This

modeling option can be useful for the simulation of radiation in combustion applications. The variable-

absorption-coefficient model used by ANSYS Fluent is the weighted-sum-of-gray-gases model (WSGGM)

described in Radiation in Combusting Flows in the Theory Guide. To activate it, first enable the species

calculation and make sure that

and

O are present in the mixture. Next, select wsggm-domain-

based, wsggm-user-specified, or user-defined-wsggm in the drop-down list to the right of Absorp-

tion Coefficient in the Create/Edit Materials dialog box. If you select user-defined-wsggm, the

User-Defined Functions dialog box will open, allowing you to select a previously loaded compiled

UDF library or a previously interpreted UDF (see Hooking DEFINE_WSGGM_ABS_COEFF UDFs in the

Fluent Customization Manual). The WSGGM options differ in the method used to compute the path

length, as described in the section that follows.

..... Path Length Inputs

When the WSGGM is used to compute the absorption coefficient, you can choose how path length,

, is defined for Equation . in the Theory Guide. See Radiation in Combusting Flows in the Theory

Guide to determine which method is appropriate for your case.

You will select the path length method when you choose the property input method for Absorption

Coefficient, as described previously.

If you choose wsggm-domain-based,  is set equal to a mean beam length calculated by ANSYS Fluent

according to Equation . in the Theory Guide, which is an average dimension of the domain; no further

inputs are required.

If you choose wsggm-user-specified,  is set equal to a mean beam length that you enter for Path

Length in the WSGGM User Specified Dialog Box (p. ).

If you choose user-defined-wsggm, ANSYS Fluent will initially compute the absorption coefficient in

the same manner as described for the wsggm-domain-based option; however, you have the option of

writing a user-defined function that customizes this calculated value. If the soot model is enabled, you

can also use the UDF to customize the soot absorption coefficient computed by ANSYS Fluent. See

DEFINE_WSGGM_ABS_COEFF in the Fluent Customization Manual for further details.

...... Inputs for a Non-Gray Radiation Absorption Coefficient

If you are using the non-gray DO model (see The DO Model Equations of the Theory Guide and De-

fining Non-Gray Radiation for the DO Model (p. )), the non-gray P- model (see The P- Model

Equations of the Theory Guide and Setting Up the P- Model with Non-Gray Radiation (p. )), or

the non-gray MC model (see Monte Carlo (MC) Radiation Model Theory), you can specify a different

constant absorption coefficient for each of the bands used by the gray-band model. Select gray-

band from the Absorption Coefficient drop-down list in the Create/Edit Materials dialog box and

then define the absorption coefficient for each band in the Gray-Band Absorption Coefficient Dialog

Box (p. ). (Note that you must complete this dialog box in order to proceed.)

...... Effect of Particles and Soot on the Absorption Coefficient

ANSYS Fluent will include the effect of particles on the absorption coefficient if you have turned on

the Particle Radiation Interaction option in the Discrete Phase Model Dialog Box (p. ) (only for

the P- and DO radiation models).

If you are modeling soot formation and you want to include the effect of soot formation on the

absorption coefficient, turn on the Soot-Radiation Interaction in the Soot Model Dialog Box (p. ).

The soot effects can be included for any of the radiation models, as long as you are using the WSGGM

to compute a composition-dependent absorption coefficient. Note that you can use the user-defined-

wsggm option to customize the soot absorption coefficient calculated by ANSYS Fluent, as described

previously.

The scattering coefficient is, by default, set to zero, and it is assumed to be isotropic. You can specify

a constant value, a temperature-dependent function (see Defining Properties Using Temperature-De-

pendent Functions (p. )), or a user-defined function. You can also specify a non-isotropic phase

function.

The scattering coefficient is requested in units of /length. Along with the absorption coefficient, it

describes the change in radiation intensity per unit length along the path through the fluid medium.

You may want to increase the scattering coefficient in combustion systems, where particulates may

be present.

.... Inputs for a Constant Scattering Coefficient

To define a constant scattering coefficient, simply enter the value in the field next to Scattering

Coefficient in the Create/Edit Materials Dialog Box (p. ). (Select constant in the drop-down list first

if it is not already selected.)

.... Inputs for the Scattering Phase Function

Scattering is assumed to be isotropic, by default, but you can also specify a linear-anisotropic scattering

function. If you are using the DO model, Delta-Eddington and user-defined scattering functions are

also available.

..... Isotropic Phase Function

To model isotropic scattering, select isotropic in the Scattering Phase Function drop-down list.

No further inputs are necessary. This is the default setting in ANSYS Fluent.

..... Linear-Anisotropic Phase Function

To model anisotropic scattering, select linear-anisotropic in the Scattering Phase Function drop-

down list and set the value of the phase function coefficient (  in Equation . in the Theory Guide).

..... Delta-Eddington Phase Function

To use a Delta-Eddington phase function, select delta-eddington in the Scattering Phase Function

drop-down list. This will open the Delta-Eddington Scattering Function Dialog Box (p. ), in which

you can specify the Forward Scattering Factor and Asymmetry Factor (  and  in Equation .

in the Theory Guide). Since this is a modal dialog box, you must tend to it immediately.

..... User-Defined Phase Function

To use a user-defined phase function, select user-defined in the Scattering Phase Function drop-

down list. The user-defined function will contain specifications for

and  in Equation . in the

Theory Guide. More information about user-defined functions can be found in the Fluent Customiz-

ation Manual.

The refractive index is the ratio of speed of light in the medium to the speed of light in vacuum. It is

by default set to . You can specify a constant value in the field next to Refractive Index.

If you are using the non-gray DO model (see The DO Model Equations of the Theory Guide and Defining

Non-Gray Radiation for the DO Model (p. )), the non-gray P- model (see The P- Model Equations

of the Theory Guide and Setting Up the P- Model with Non-Gray Radiation (p. )), or the non-gray

MC model (see Monte Carlo (MC) Radiation Model Theory), you can specify a different constant refractive

index for each of the bands used by the gray-band model. Select refractive-band from the Refractive

Index drop-down list in the Create/Edit Materials dialog box and then define the refractive index for

each band in the Gray-Band Refractive Index Dialog Box (p. ). Note that because this is a modal

dialog box, you must tend to it immediately.

You can display the computed local values for  and

using the Absorption Coefficient and Scat-

tering Coefficient items in the Radiation... category of the variable selection drop-down list that ap-

pears in postprocessing dialog boxes. You will also find the Refractive Index in the Radiation... cat-

egory.

For species transport calculations, there are two ways to model the diffusion of chemical species. For

most applications the Fick’s law approximation is adequate, but for some applications (for example,

diffusion-dominated laminar flows such as chemical vapor deposition), the full multicomponent diffusion

model is recommended.

Important

The full multicomponent diffusion model is enabled in the Species Model Dialog Box (p. )

and is computationally expensive.

... Fickian Diffusion

... Full Multicomponent Diffusion

... Anisotropic Species Diffusion

...Thermal Diffusion Coefficients

... Mass Diffusion Coefficient Inputs

... Mass Diffusion Coefficient Inputs for Turbulent Flow

Mass diffusion coefficients are required whenever you are solving species transport equations in mul-

ticomponent flows. Mass diffusion coefficients are used to compute the diffusion flux of a chemical

species in a laminar flow using (by default) Fick’s law:

(.)

where

is the mass diffusion coefficient for species  in the mixture and

is the thermal (Soret)

diffusion coefficient.

Equation . (p. ) is strictly valid when the mixture composition is not changing, or when

is

independent of composition. This is an acceptable approximation in dilute mixtures when

, for

all  except the carrier gas. ANSYS Fluent can also compute the transport of non-dilute mixtures in

Mass Diffusion Coefficients

laminar flows by treating such mixtures as multicomponent systems. Within ANSYS Fluent,

can

be specified in a variety of ways, including by specifying

, the binary mass diffusion coefficient of

component  in component .

is not used directly, however; instead, the diffusion coefficient in

the mixture,

, is computed as

(.)

where

is the mole fraction of species . You can input

or

for each chemical species, as de-

scribed in Mass Diffusion Coefficient Inputs (p. ).

In turbulent flows, Equation . (p. ) is replaced with the following form:

(.)

where

is the effective Schmidt number for the turbulent flow:

(.)

and

is the effective mass diffusion coefficient due to turbulence.

(.)

where

(.)

and

In turbulent flows your mass diffusion coefficient inputs consist of defining the molecular contribution

to diffusion

using the same methods available for the laminar case, with the added option to alter

the default settings for the turbulent Schmidt number. As seen from Equation . (p. ), this para-

meter relates the effective mass diffusion coefficient due to turbulence with the eddy viscosity

. As

discussed in Mass Diffusion Coefficient Inputs for Turbulent Flow (p. ), the turbulent diffusion coef-

ficient normally overwhelms the laminar diffusion coefficient, so the default constant value for the

laminar diffusion coefficient is usually acceptable.

A careful treatment of chemical species diffusion in the species transport and energy equations is im-

portant when details of the molecular transport processes are significant (for example, in diffusion-

dominated laminar flows). As one of the laminar-flow diffusion models, ANSYS Fluent has the ability

to model full multicomponent species transport.

.... General Theory

For multicomponent systems it is not possible, in general, to derive relations for the diffusion fluxes

containing the gradient of only one component (as described in Fickian Diffusion (p. )). Here, the

Maxwell-Stefan equations will be used to obtain the diffusive mass flux. This will lead to the definition

of generalized Fick’s law diffusion coefficients  [] (p. ). This method is preferred over computing

the multicomponent diffusion coefficients since their evaluation requires the computation of

co-

factor determinants of size

, and one determinant of size

co-

[] (p. ), where

is the number of chemical species.

.... Maxwell-Stefan Equations

From Merk  [] (p. ), the Maxwell-Stefan equations can be written as

(.)

where,

= the mole fraction

= the diffusion velocity

= the binary mass diffusion coefficient of species  in species

= the thermal diffusion coefficient.

For an ideal gas the Maxwell diffusion coefficients are equal to the binary diffusion coefficients. If the

external force is assumed to be the same on all species and that pressure diffusion is negligible, then

. Since the diffusive mass flux vector is

, the above equation can be written as

(.)

After some mathematical manipulations, the diffusive mass flux vector,

, can be obtained from

(.)

where

is the mass fraction of species . Other terms are defined as follows:

(.)

where,

and

=

matrices

= an

matrix of the generalized Fick’s law diffusion coefficients

[] (p. )

= the molecular weight

= a subscript used to define a mean molecular weight in the mixture

You can model anisotropic species diffusion in porous media.

For Fickian diffusion, the mass flux vector of species  is modeled as,

(.)

where  is the porosity,

is the anisotropic diffusion matrix in the porous zone, and the remaining

nomenclature is the same as in Equation . (p. ).

The Full Multi-component (Maxwell-Stefan) anisotropic diffusion flux vector is calculated similar to

Equation . (p. ) as,

(.)

To account for anisotropic species diffusion in porous media simulations, select the Anisotropic Species

(.)

Diffusion check box in the Porous Zone tab of the Fluid dialog box and specify the Matrix Compon-

ents for the anisotropic diffusion matrix

(see Figure . : Anisotropic Species Diffusion Matrix (p. )).

Figure . : Anisotropic Species Diffusion Matrix

By default,

is the identity matrix that corresponds to isotropic diffusion.

The thermal diffusion coefficients can be defined as constants, polynomial functions, user-defined

functions, or using the following empirically-based composition-dependent expression derived from

[] (p. ):

(.)

This form of the Soret diffusion coefficient will cause heavy molecules to diffuse less rapidly, and light

molecules to diffuse more rapidly, towards heated surfaces.

....Thermal Diffusion Coefficient Inputs

If you have enabled thermal diffusion (in the Species Model Dialog Box (p. )), you can define the

thermal diffusion coefficients in the Create/Edit Materials Dialog Box (p. ) as follows:

. Select one of the following three methods in the drop-down list to the right of Thermal Diffusion

Coefficient:

Choose kinetic-theory to have ANSYS Fluent compute the thermal diffusion coefficients using the

empirically-based expression in Equation . (p. ). No further inputs are required for this option.

Choose specified to input the coefficient for each species.The Thermal Diffusion Coefficients Dialog

Box (p. ) (Figure . :The Thermal Diffusion Coefficients Dialog Box (p. )) will open. Further inputs

are described in the step .

Choose user-defined to use a user-defined function. More information about user-defined functions

. (specified method only) For each species in the Species Thermal Di list of the Thermal Diffusion

Coefficients dialog box, perform the following steps:

Figure . : The Thermal Diffusion Coefficients Dialog Box

a.

Select the species in the Species Thermal Di list for which you are going to define the thermal diffusion

coefficient.

b. Define

for the selected species either as a constant value or as a polynomial function of temper-

ature:

To define a constant diffusion coefficient, select constant (the default) in the drop-down list below

Coefficient, and then enter the value in the field below the list.

To define a temperature-dependent diffusion coefficient, choose polynomial in the Coefficient

drop-down list and then define the polynomial coefficients as described in Defining Properties

By default, the solver computes the species diffusion using Equation . (p. ) (for laminar flows)

with your inputs for

, the diffusion coefficient for species  in the mixture. For turbulent flows,

species diffusion is computed with Equation . (p. ).

You can input the mass diffusion coefficients using one of the following methods:

Constant dilute approximation (Fickian diffusion only): define one constant for all

.

Dilute approximation (Fickian diffusion only): define each

as a constant or as a polynomial function of

temperature (if heat transfer is enabled).

Multicomponent method: define the binary diffusion of species  in each species ,

as a constant or a

polynomial function of temperature, or (for ideal gases only) using kinetic theory.

Unity Lewis Number: define

under the assumption of unity Lewis number for all species in the mixture.

User-defined function (UDF): define a single function that will apply to all mass diffusion coefficients.This

is done using the DEFINE_DIFFUSIVITY macro and is explained in the Fluent Customization Manual.

You should choose to input

(using one of the first two methods) if you are modeling a dilute

mixture, with chemical species present at low mass fraction in a “carrier” fluid that is present at high

concentration. You may want to define the individual binary mass diffusion coefficients,

, if you are

modeling a non-dilute mixture. If you choose to define

, the solver will compute the diffusion of

species  in the mixture using Equation . (p. ), unless you have enabled full multicomponent

diffusion.

The Lewis number is the ratio of thermal diffusivity (Prandtl number) to mass diffusivity (Schmidt

number). Flames with non-unity Lewis number can display instabilities, as well as non-adiabatic flame

temperatures. The Unity Lewis Number mass diffusivity option avoids these issues, and is particularly

appropriate for the Thickened Flame model.

Important

If you want to use the full multicomponent diffusion model described in Full Multicomponent

Diffusion (p. ), turn on the Full Multicomponent Diffusion option in the Species Model

Dialog Box (p. ), and then select the multicomponent diffusion model.

You will define

or

or

for each chemical species using the Create/Edit Materials Dialog Box (p. ).

Setup →

Materials

The diffusion coefficients have units of

/s in SI units or

/s in British units.

.... Constant Dilute Approximation Inputs

To use the constant dilute approximation method, follow these steps:

. Select constant-dilute-appx in the drop-down list to the right of Mass Diffusivity.

. Enter a single value of

.The same value will be used for the diffusion coefficient of each species in

the mixture.

.... Dilute Approximation Inputs

To use the dilute approximation method, follow the steps below:

. Select dilute-approx in the drop-down list to the right of Mass Diffusivity.

. In the resulting Mass Diffusion Coefficients Dialog Box (p. ) (Figure . :The Mass Diffusion Coefficients

Dialog Box for Dilute Approximation (p. )), select the species in the Species Di list for which you are

going to define the mass diffusion coefficient.

Figure . : The Mass Diffusion Coefficients Dialog Box for Dilute Approximation

. You can define

for the selected species either as a constant value or (if heat transfer is active) as a

polynomial function of temperature:

To define a temperature-dependent diffusion coefficient, choose polynomial in the Coefficient drop-

down list and then define the polynomial coefficients as described in Inputs for Polynomial Func-

(.)

(.)

. Repeat steps  and  until you have defined diffusion coefficients for all species in the Species Di list in

the Mass Diffusion Coefficients Dialog Box (p. ).

.... Multicomponent Method Inputs

To use the multicomponent method, and define constant or temperature-dependent diffusion coeffi-

cients, follow the steps below:

. Select multicomponent in the drop-down list to the right of Mass Diffusivity.

Dialog Box for the Multicomponent Method (p. )), select the species in the Species Di list and the

Species Dj list for which you are going to define the mass diffusion coefficient

for species  in species

.

Figure . : The Mass Diffusion Coefficients Dialog Box for the Multicomponent Method

for the selected pair of species as a constant value or as a polynomial function of

temperature (if heat transfer is active).

(.)

. Repeat steps  and  until you have defined diffusion coefficients for all pairs of species in the Species

Di and Species Dj lists in the Mass Diffusion Coefficients Dialog Box (p. ).

To use the multicomponent method, and define the diffusion coefficient using kinetic theory (available

only when the ideal gas law is used), follow these steps:

. Choose kinetic-theory in the drop-down list to the right of Mass Diffusivity.

. Click Change/Create after completing other property definitions for the mixture material.

. Define the Lennard-Jones parameters,

and

, for each species (fluid material), as described in

Kinetic Theory Parameters (p. ).

The solver will use a modification of the Chapman-Enskog formula  [] (p. ) to compute the diffusion

coefficient using kinetic theory:

(.)

where,

is the absolute pressure

is the diffusion collision integral, which is a measure of the interaction of the

molecules in the system

is a function of the quantity

, where

(.)

is the Boltzmann constant, which is defined as the gas constant,

, divided by Avogadro’s number.

for the mixture is the geometric average:

(.)

For a binary mixture,

is calculated as the arithmetic average of the individual s:

(.)

.... Unity Lewis Number

The laminar mass diffusivity of all species is calculated as:

where

denotes the mass diffusivity of species  in the mixture,

is the thermal conductivity,

is the mixture density, and

is the mixture specific heat.

When your flow is turbulent, you will define

or

, as described for laminar flows in Mass Diffusion

Coefficient Inputs (p. ), and you will also have the option to alter the default setting for the turbulent

Schmidt number,

, as defined in Equation . (p. ).

Usually, in a turbulent flow, the mass diffusion is dominated by the turbulent transport as determined

by the turbulent Schmidt number (Equation . (p. )). The turbulent Schmidt number measures

the relative diffusion of momentum and mass due to turbulence and is on the order of unity in all

turbulent flows. Because the turbulent Schmidt number is an empirical constant that is relatively in-

sensitive to the molecular fluid properties, you will have little reason to alter the default value (.)

for any species.

Should you want to modify the Schmidt number, enter a new value for Turb. Schmidt Number in the

Viscous Model Dialog Box (p. ).

Edit...

Important

Note that the full multicomponent diffusion model described in Full Multicomponent Diffu-

sion (p. ) is not recommended for turbulent flows.

When you are solving a reacting flow using the finite-rate or eddy dissipation model, you must define

the standard state enthalpy (also known as the formation enthalpy or heat of formation),

for each

species . These inputs are used to define the mixture enthalpy as

(.)

where

is the molecular weight of the

th species with units of kg/kmol and

is the reference

temperature at which

is defined. Standard state enthalpies are input in units of J/kg mol in SI units

or in units of Btu/

mol in British units.

For each species involved in the reaction (that is, each fluid material contained in the mixture material),

you can set the Standard State Enthalpy and Reference Temperature in the Create/Edit Materials

If you are using the finite-rate model with reversible reactions (see Direct Use of Finite-Rate Kinetics

(no TCI) in the Theory Guide), you must define the standard state entropy,

for each species . These

inputs are used to define the mixture entropy as

(.)

where

is defined. Standard state entropies are input in units of J/kmol-K in SI units

mol-°R in British units.

you can set the Standard State Entropy and Reference Temperature in the Create/Edit Materials

If you are modeling premixed combustion (see Modeling Premixed Combustion (p. )), the fluid ma-

terial in your domain should be assigned the properties of the unburnt mixture, including the thermal

diffusivity (  in Equation . in the Theory Guide).

, and values at standard con-

ditions can be found in combustion handbooks (for example, [] (p. )). To determine values at non-

standard conditions, you must use a third-party 1D combustion program with detailed chemistry. You

can set the Unburnt Thermal Diffusivity in the Create/Edit Materials Dialog Box (p. ).

You may choose to define the following properties using kinetic theory when the ideal gas law is enabled:

viscosity (for fluids)

thermal conductivity (for fluids)

specific heat capacity (for fluids)

mass diffusion coefficients (for multi-species mixtures)

If you are using kinetic theory for a fluid’s viscosity (Equation . (p. )), you must input the kinetic

theory parameters  and

for that fluid. These parameters are the Lennard-Jones parameters and

are referred to by ANSYS Fluent as the “characteristic length” and the “energy parameter” respectively.

When kinetic theory is applied to calculation of a fluid’s thermal conductivity only, no inputs are required.

To calculate specific heat of a fluid using kinetic theory (Equation . (p. )), you need to enter the degrees

of freedom for the fluid material.

If you use kinetic theory to define a mixture material’s mass diffusivity (Equation . (p. )), you must input

and

for each chemical species .

Kinetic Theory Parameters

... Inputs for Kinetic Theory

The procedure for using kinetic theory is as follows:

. Select kinetic-theory as the property specification method for the Viscosity, Thermal Conductivity, or

heat capacity Cp of a fluid material, or for the Mass Diffusivity of a mixture material.

. If the material for which you have selected the kinetic theory method for one or more properties is a fluid

material, you must set the kinetic theory parameters for each of the constituent species (fluid materials).

The parameters to be set are as follows:

L-J Characteristic Length

L-J Energy Parameter

Degrees of Freedom (only required if kinetic theory is used for specific heat)

See the beginning of this section to find out which parameters are required to calculate each

property using kinetic theory.

Characteristic length is defined in units of Angstroms. The energy parameter is defined in units of ab-

solute temperature. Degrees of freedom is a dimensionless input. All kinetic theory materials can be

found in the literature (for example, [] (p. )).

Specification of the operating pressure affects your calculation in different ways for different flow regimes.

This section presents information about the operating pressure, its relevance for different cases, and

how to set it correctly.

...The Significance of Operating Pressure

... Operating Pressure, Gauge Pressure, and Absolute Pressure

... Setting the Operating Pressure

Operating pressure is significant for incompressible ideal gas flows because it directly determines the

density: the incompressible ideal gas law computes density as

. You must therefore be sure to

set the operating pressure appropriately.

In low-Mach-number compressible flow, the overall pressure drop is small compared to the absolute

static pressure, and can be significantly affected by numerical roundoff. To understand why this is true,

consider a compressible flow with

. The pressure changes,

, are related to the dynamic head,

, where  is the static pressure and  is the ratio of specific heats. This gives the simple relation-

ship

, so that

as

. Therefore, unless adequate precaution is taken, low-

Mach-number flow calculations are very susceptible to roundoff error.

ship

, so that

as

Operating pressure is significant for low-Mach-number compressible flows because of its role in

avoiding roundoff error problems. Ensure that you set the operating pressure appropriately. You may

want to specify a floating operating pressure instead of a constant operating pressure for low-Mach-

number, time-dependent compressible flows with average pressure in the domain varying in time. See

Floating Operating Pressure (p. ) for details.

Operating pressure is less significant for higher-Mach-number compressible flows. The pressure changes

in such flows are much larger than those in low-Mach-number compressible flows, so there is no real

problem with roundoff error and, therefore, no real need to use gauge pressure. In fact, it is common

convention to use absolute pressures in such calculations. Since ANSYS Fluent always uses gauge

pressure, you can simply set the operating pressure to zero, making gauge and absolute pressures

If the density is assumed constant or if it is derived from a profile function of temperature, the operating

pressure is not used in the density calculation.

Note that the default operating pressure is  Pa.

ANSYS Fluent avoids the problem of roundoff error (discussed in The Significance of Operating Pres-

sure (p. )) by subtracting the operating pressure (generally a large pressure roughly equal to the

average absolute pressure in the flow) from the absolute pressure, and using the result (termed the

gauge pressure). The relationship between the operating pressure, gauge pressure, and absolute

pressure is shown below. The absolute pressure is simply the sum of the operating pressure and the

gauge pressure:

(.)

All pressures that you specify and all pressures computed or reported by ANSYS Fluent are gauge

pressures.

The criteria for choosing a suitable operating pressure are based on the Mach-number regime of the

flow and the relationship that is used to determine density. For example, if you use the ideal gas law

in an incompressible flow calculation (for example, for a natural convection problem), you should use

a value representative of the mean flow pressure.

To place this discussion in perspective, Table . : Recommended Settings for Operating Pressure (p. )

shows the recommended approach for setting operating pressures. The default operating pressure is

Pa.

Table . : Recommended Settings for Operating Pressure

Operating Pressure

Mach Number Regime

Density Relationship

or

mean flow pressure

ideal gas law

not used

incompressible

profile function of temperature

not used

constant

incompressible ideal gas law

You will set the Operating Pressure in the Operating Conditions Dialog Box (p. ).

Setup →

For incompressible flows that do not involve any pressure boundaries, ANSYS Fluent adjusts the gauge

pressure field after each iteration to keep it from floating. This is done using the pressure in the cell

located at (or nearest to) the reference pressure location. The pressure value in this cell is subtracted

from the entire gauge pressure field; as a result, the gauge pressure at the reference pressure location

is always zero. If pressure boundaries are involved, the adjustment is not needed and the reference

pressure location is ignored.

The reference pressure location is, by default, the cell center at or closest to (,,). There may be cases

in which you might want to move the reference pressure location, perhaps locating it at a point where

the absolute static pressure is known (for example, if you are planning to compare your results with

experimental data). To change the location, enter new (X,Y,Z) coordinates for Reference Pressure

Location in the Operating Conditions Dialog Box (p. ).

Setup →

... Actual Reference Pressure Location

For cases that do not have pressure-related boundary conditions (for example, pressure inlet, pressure

outlet, pressure far-field, and so on), you need to specify the Reference Pressure Location at a point

in the problem domain. Internally, ANSYS Fluent sets the location of the reference pressure at a slightly

different nearby location. Therefore, the actual location used as the pressure reference is different than

that of your input value. To report the actual reference pressure location that ANSYS Fluent uses, use

the following text command:

define → operating-conditions → used-ref-pressure-location

Important

Important

This text command is available only when the case is initialized and has no pressure-related

boundary zones.

Reporting the actual reference pressure location is not available through the graphical user in-

terface.

Some engineering problems involve fluids that do not behave as ideal gases. For example, at very high-

pressure or very low-temperature conditions (for example, the flow of a refrigerant through a compressor)

the flow cannot typically be modeled accurately using the ideal-gas assumption. Therefore, the real gas

model allows you to solve accurately for the fluid flow and heat transfer problems where the working

fluid behavior deviates from the ideal-gas assumption.

ANSYS Fluent provides three real gas options for solving these types of flows:

Cubic Equation of State Models (p. )

The NIST Real Gas Models (p. )

The User-Defined Real Gas Model (p. )

All the models allow you to solve for either a single-species fluid flow or a multiple-species mixture

fluid flow.

... Choosing a Real Gas Model

... Cubic Equation of State Models

...The NIST Real Gas Models

...The User-Defined Real Gas Model

The states at which a pure material can exist can be graphically represented in diagrams of pressure

vs. temperature (PT diagrams) and pressure vs. molecular or specific volume (PV diagrams). Homogen-

eous fluids are normally divided into two classes, liquids and gases. However the distinction cannot

always be sharply drawn, because the two phases become indistinguishable at what is called the crit-

ical point. A typical pressure-temperature (PT) diagram of a pure material is shown in Figure . : Typ-

ical PT Diagram of a Pure Material (p. ).

Figure . : Typical PT Diagram of a Pure Material

This figure shows the single phase regions, as well as the conditions of P and T where two phases

coexist. Therefore the solid and the gas region are divided by the sublimation curve, the liquid and

gas regions by the vaporization curve, and the solid and liquid regions by the fusion curve. The three

curves meet at the triple point, where all three phases coexist in equilibrium. Although the fusion

Real Gas Models

curve continues upward indefinitely, the vaporization curve terminates at the critical point. The coordin-

ates of this point are called the critical pressure

and critical temperature

. These represent the

highest temperature and pressure at which a pure material can exist in vapor-liquid equilibrium. At

temperatures and pressures above the critical point, the physical property differences that differentiate

the liquid phase from the gas phase become less defined. This reflects the fact that, at extremely high

temperatures and pressures, the liquid and gaseous phases become indistinguishable. This new phase,

which has some properties that are similar to a liquid and some properties that are similar to a gas, is

called a supercritical fluid.

Figure . : Typical PV Diagram of a Pure Material

Figure . : Typical PV Diagram of a Pure Material (p. ) presents a typical diagram of pressure versus

molar or specific volume (PV diagram) of a pure material. The dome shaped curve ACD is called the

saturation dome and separates the single phase regions in the diagram; curve AC represents the sat-

urated liquid and curve CD the saturated vapor. The area under the saturation dome ACD is the two-

phase region and represents all possible mixtures of vapor and liquid in equilibrium. Curve ECB is the

critical isotherm and exhibits a horizontal inflection at point C at the top of the dome. This is the crit-

ical point. The specific volume corresponding to the critical point, is called the critical specific volume

. The conditions to the right of the critical isotherm ECB correspond to supercritical fluid. The dashed

lines CF and CG in Figure . : Typical PV Diagram of a Pure Material (p. ) represent the liquid and

the vapor spinodal curves with the regions ACF and DCG between the saturation and spinodal lines

representing the superheated liquid and supercooled vapor states, respectively. These states are called

"metastable" because they exist temporarily in small local regions until phase change occurs. As an

example, liquid metastable states may be formed in situations of fast depressurization, depending on

the rate of depressurization and the disturbances that tend to make the liquid flash into vapor.

The equation of state is the mathematical expression that relates pressure, molar or specific volume,

and temperature for any pure homogeneous fluid in equilibrium states.

The simplest equation of state is the ideal gas law, which is approximately valid for the low pressure

gas region of the PT and PV diagrams. Ideal gas behavior can be expected when

or

and

or

and

If your flow conditions correspond to either of those cases, you may use the ideal gas law in your

simulation.

Another idealization, that of the incompressible fluid, can be employed for the low pressure region of

the liquid phase. A constant density option is the appropriate selection in that case.

However, both of these approaches are not good approximations for flow conditions close to and

beyond the critical point, where the fluid behavior cannot be described by the ideal gas, or the incom-

pressible liquid assumptions. We refer to a fluid under those conditions as a real fluid, or a real gas

and more complex relations are used for the determination of its physical and thermodynamic prop-

erties.

ANSYS Fluent provides the following options for solving real fluid problems:

The cubic equation of state models can be used to solve problems in the gas, liquid, and supercritical fluid

regimes.The models are not available for the two-phase region under the phase dome. For further details

see Cubic Equation of State Models (p. ).

The NIST real gas model can be used to solve problems in the liquid, or gas and supercritical fluid regimes.

The model does not allow modeling of the two-phase region. For further details see The NIST Real Gas

Models (p. ).

The user-defined real gas model allows you to solve problems in all regimes, as long as appropriate rela-

tionships are provided through the user-defined real gas functions. For further details see The User-Defined

Real Gas Model (p. ).

The concepts presented in this section for pure materials are also extended to multicomponent mixtures

with the introduction of appropriate composition-dependent parameters in the real gas equations of

state and the material property models. All the real-gas modeling options above allow for either single-

species or multicomponent flow modeling. In addition, you may solve reacting flow problems with

the cubic equations of state models and the user-defined real gas functions.

.... Overview and Limitations

An equation of state is a thermodynamic equation, which provides a mathematical relationship

between two or more state functions associated with the matter, such as its temperature, pressure,

volume, or internal energy. One of the simplest equations of state for this purpose is the ideal gas

law, which is roughly accurate for gases at low pressures and high temperatures. However, this

equation becomes increasingly inaccurate at higher pressures and lower temperatures, and fails to

predict condensation from a gas to a liquid.

Introduced in , the Redlich-Kwong equation of state  [] (p. ) was a considerable improvement

over other equations of that time. It is an analytic cubic equation of state and is still of interest

primarily due to its relatively simple form. The original form is

(.)

where

P = absolute pressure (Pa)

R = universal gas constant

V = specific molar volume (

)

T = temperature (K)

= reduced temperature

, where

is the critical temperature

and  are constants related directly to the fluid critical pressure and temperature

)

, where

Many investigators have attempted to improve the accuracy of the Redlich-Kwong equation. ANSYS

Fluent has adopted the original form of the Redlich-Kwong equation, as well as the following modified

forms:

The Soave-Redlich-Kwong [] (p. ) equation is a three-parameter equation of state, which can be

applied for vapor, supercritical, and liquid property predictions. It has found wide acceptance mainly in

the oil and gas industry and requires knowledge of the critical temperature, critical pressure, and acentric

factor. It was developed by replacing the Redlich-Kwong attractive coefficient defined as

with

a two-parameter form

, where

is the acentric factor.

The Peng-Robinson equation [] (p. ) is a three-parameter equation of state, also requiring the critical

temperature, critical pressure and acentric factor parameters. It is thought to perform as well as the Soave-

Redlich-Kwong equation, with an advantage in the prediction of the liquid densities.

The Aungier-Redlich-Kwong [] (p. ) equation provides improved predictions for vapor and supercritical

fluids near the critical point, as well as for materials with a negative value of the acentric factor.The

Aungier modified form is a four parameter equation and requires the critical specific volume in addition

to the critical temperature, critical pressure and acentric factor.

The following limitations exist in ANSYS Fluent for all cubic equation of state models:

Pressure-inlets, mass flow-inlets, and pressure-outlets are the only inflow and outflow boundaries available

for use with the real gas models.

Non-reflecting boundary conditions are not compatible with the real gas models when using the density-

based solver. If your model requires NRBC and a real gas model, you must use the pressure-based solver.

The cubic equation of state real gas models are compatible with the Eulerian multiphase models.

The cubic equation of state models are compatible with the Lagrangian Dispersed Phase Models. If you

are modeling droplet or multicomponent particles, note that the current formulation does not take into

account the near-critical point phenomena, which means that accurate results can be obtained for droplet

temperatures below

. See Using the Cubic Equation of State Models with the Lagrangian Dis-

persed Phase Models (p. ) for more details.

The real gas models are not available with the premixed, inert, and composition PDF transport combustion

models.

The cubic equation of state real gas models can be used with the following species models:

– Species transport. Chemical reactions can be modeled with the finite rate and eddy dissipation models.

Note that the Dimension Reduction model is not available with the real gas models.

– Non-premixed model and partially-premixed model. Note that the Compressibility Effects option

must be enabled in the Species Model dialog box in order for the real-gas models to be available. In

addition the following restrictions apply when the non-premixed model is used together with a cubic

equation of state real-gas model:

→ The empirical stream options cannot be used, as for the empirical species the critical properties

cannot be defined.

→ Condensed species such as h2o<l> and c<s> are not supported and should be excluded from the

PDF table, so ensure that you add all condensed species for your system in the excluded species list

prior to the PDF table generation.

The laminar flame speeds for the partially-premixed model are assumed to be the same as for ideal-

gases.

When the cubic equation of state models are applied for subcritical conditions near or under the phase

dome, the two-phase flow is not modeled and either vapor or liquid state must be selected. Subcritical

and supercritical states can co-exist in the same simulation.

.... Equation of State

The general form of pressure P for the cubic equation of state models is written as [] (p. ) :

(.)

where

)

The coefficients ,

, ,

, and  are given for each equation of state as functions of the critical

, critical pressure

, acentric factor

and critical specific volume

. Note that the

attractive coefficient  also has a temperature dependence, which varies for each equation of state

model, and is commonly written as

.

Redlich-Kwong Equation [] (p. ):

(.)

(.)

(.)

The parameter  is set equal to , while  and  are set to . The Redlich-Kwong equation is the

simplest of the cubic equations of state in ANSYS Fluent and requires two parameters only, the critical

and the critical pressure

.

Soave-Redlich-Kwong Equation [] (p. ):

(.)

(.)

and  are given by Equation . (p. ) and Equation . (p. ) respectively. As in the original

.

(.)

(.)

Redlich-Kwong equation the parameter  is set equal to , while  and  are set to . The Soave-

Redlich-Kwong requires three parameters, the critical temperature

, the critical pressure

, and

the acentric factor

.

Peng-Robinson Equation [] (p. ):

(.)

(.)

The function

is given by Equation . (p. ), with n provided in Equation . (p. ) as follows:

(.)

In the Peng-Robinson equation  is set equal to

,  is equal to

, and  is set to .

Similar to the Soave-Redlich-Kwong equation, the Peng-Robinson equation is a three-parameter

equation and requires the critical temperature

, and the acentric factor

.

Aungier-Redlich-Kwong Equation [] (p. ):

(.)

(.)

and  are given by Equation . (p. ) and Equation . (p. ), respectively. As in the original

Redlich-Kwong equation, the parameter  is set equal to  and  is set to . Parameter  is given by:

(.)

The Aungier-Redlich-Kwong equation requires four parameters, namely the critical temperature

,

the critical pressure

, the critical specific volume

.

.... Enthalpy, Entropy, and Specific Heat Calculations

Enthalpy, entropy, and specific heat are computed in terms of the relevant ideal gas properties and

the departure functions. The departure function

of any conceptual property  is defined as

[] (p. )

(.)

where

is the value of the property as computed from the ideal gas relations. The departure

function

can be derived from basic thermodynamic relations and the equation of state.

Following the above definition, the enthalpy

function

for the equations of state models is given by the fol-

lowing equations  [] (p. ):

(.)

(.)

(.)

where,

= ideal gas enthalpy at temperature T (J/kg)

= departure enthalpy (J/kmol)

= mean molecular weight (Kg/kmol)

= pressure (Pa)

= specific molar volume (

/kmol)

= universal gas constant

,

, and  are computed using Equation . (p. )– Equation . (p. ) depending

on the equation of state model

See Equation . (p. ) for a description of other coefficients.

Similarly, the departure internal energy

can be shown to be

(.)

where

= departure internal energy (J/kmol)

= temperature (K)

/kmol)

is given by Equation . (p. )

,

, and  are computed using Equation . (p. ) – Equation . (p. ) depending

The specific heat

can be computed from the ideal specific heat

and the departure specific

heat at constant volume

(.)

(.)

where

= mean molecular weight (kg/kmol)

/kmol)

In Equation . (p. )

is computed by differentiating the equation of departure internal energy

(Equation . (p. )) with respect to

, and the partial derivatives of the specific volume are

computed by differentiating Equation . (p. ) appropriately.

The entropy  is computed by

(.)

(.)

where

= ideal gas entropy at temperature T and reference pressure (J/kg/K)

= ideal gas specific molar volume at temperature T and the reference

pressure (

/kmol)

/kmol)

pressure (

/kmol)

/kmol)

is given by Equation . (p. ) and ,

, and  are computed using Equation . (p. ) –

Equation . (p. ), depending on the equation of state model. Note that the pressure term in

Equation . (p. ) cancels out as both

and

are evaluated at the reference pressure.

.... Critical Constants for Pure Components

Equations describing real-gas properties require the knowledge of the critical constants for pure

components and mixtures. These consist of the critical temperature (

), critical pressure (

), critical

specific volume (

), and the acentric factor (

).

Several critical constants for fluid materials in the ANSYS Fluent property database propdb.scm

have been compiled from a variety of sources available in the open literature  [] (p. ), [] (p. ),

[] (p. ), [] (p. ), [] (p. ), [] (p. ), [] (p. ).

For those fluid materials, for which the critical properties have not been found in the open literature,

these have been estimated using the commercially available software CRANIUM by Molecular Know-

ledge Systems Inc. [] (p. ) : http://www.molknow.com/Cranium/cranium.htm

Critical property values for many hydrocarbon and nitrogenous radical species have been obtained

from Tang and Brezinsky [] (p. ). Where the critical properties for the radicals were not available

in the literature, these were estimated using a modification of the Joback method [] (p. ). This

assumes that the radical site constitutes a distinct group with zero group contribution and utilizes

the group contribution values for stable species.

The critical properties of coal volatiles have been estimated assuming that the volatiles can be approx-

imated by a mixture of CO,

,

,

, and

in such a way, that the atom composition and

the net calorific value of the volatiles is similar to that of the assumed mixture. The critical properties

of the lignite and biomass volatiles have been assumed equal to those of formaldehyde. The critical

properties of diesel and jet-a fuels have been set equal to those of decane. The critical properties of

kerosene have been set equal to those of dodecane.

.... Calculations for Mixtures

For the computation of properties in real-gas mixtures, ANSYS Fluent follows the so-called pseudocrit-

ical method. According to this method, the behavior and properties of a real gas mixture will be the

same as that of a pure component, to which appropriate critical constants are assigned. These mixture

critical constants are functions of the mixture composition and pure component critical properties,

and are sometimes called pseudocritical constants, because their values are generally expected to be

different from the true mixture critical constants that may be determined experimentally. However

for computational purposes they are the appropriate critical constant values for the mixture. According

to the pseudocritical method, ANSYS Fluent applies Equation . (p. )– Equation . (p. ) also

for mixtures, where the critical temperature

, critical specific volume

, and

acentric factor

, are replaced by the corresponding mixture critical constants, critical temperature

, and

, and acentric factor

.

The following options are available in ANSYS Fluent for the calculation of the mixture pseudocritical

constants:

The simplest rule for computing the pseudocritical constants

for a real gas mixture is the mole fraction

average  [] (p. ).This method is recommended for mixtures where the pure component critical

properties for all components are not very different:

(.)

where

= mixture pseudocritical constant (temperature, pressure, specific volume or acentric factor)

= critical constant of component i (temperature, pressure, specific volume or acentric factor)

= mole fraction of component i

= number of components in mixture

An alternative approach is based on the one-fluid van der Waals mixing rules as expressed in [] (p. ).

According to this approach, in order to apply the equation of state models to mixtures, the coefficients

and  in Equation . (p. ) are replaced by composition-dependent expressions as follows:

(.)

(.)

where

= mole fraction of species i

With the appropriate expressions from Equation . (p. )– Equation . (p. ) for each

equation of state, and assuming a mixture acentric factor

for the evaluation of parameter  in

Equation . (p. ), Equation . (p. ), and Equation . (p. ), the mixing rules Equa-

tion . (p. ) and Equation . (p. ) can be rearranged to yield direct expressions of the

mixture critical properties as functions of the mole fractions and the component critical properties

[] (p. ).

The resulting expressions for the mixture critical specific temperature

[] (p. ).

– Soave-Redlich-Kwong and Peng-Robinson models

(.)

– Redlich-Kwong model and Aungier-Redlich-Kwong model:

(.)

where for the Aungier-Redlich-Kwong model  is obtained from Equation . (p. ) as function

of the mixture acentric factor

. For the Redlich-Kwong model

.

The mixture critical specific pressure

is computed as:

(.)

The mixture critical specific volume

(.)

The notation for Equation . (p. ) to Equation . (p. ) is

= mixture pseudocritical temperature (K)

= mixture pseudocritical pressure (Pa)

= mixture pseudocritical molar volume (

/kmol)

= critical temperature for component i (K)

= critical pressure for component i (Pa)

= critical molar volume for component i (

/kmol)

= mole fraction for component i

..... Using the Cubic Equation of State Real Gas Models

For single or multicomponent flows, you will enable the cubic equation of state real gas models by

selecting real-gas-soave-redlich-kwong, real-gas-peng-robinson, real-gas-aungier-redlich-kwong,

or real-gas-redlich-kwong from the Density drop-down list in the Create/Edit Materials dialog

box.

Setup →

The required inputs for the cubic equation of state real gas models for single component flow and

mixtures are described below.

Single Component Flow

Figure . : The Cubic Equation of State Model for a Real-Gas Fluid

When any of the cubic equation of state models is enabled, enter the following material properties

in the dialog box:

ideal specific heat

molecular weight

standard state entropy

reference temperature

critical temperature

critical pressure

critical specific volume

Important

Your inputs for the specific heat in the Materials dialog box will now be used to compute

the ideal property functions

,

, and

in Equation . (p. ), Equa-

tion . (p. ), and Equation . (p. ), respectively. In ANSYS Fluent the departure

properties will be computed and added to the ideal part, to yield the real gas specific

heat, enthalpy, and entropy.

Mixtures

Figure . : The Cubic Equation of State Model for a Real-Gas Mixture

When one of the cubic equation of state models is selected from the Density drop-down list, specify

the following material properties for the mixture material in the dialog box:

You also need to enter the following material properties for each of the mixture components in the

dialog box:

When you are modeling a real-gas mixture, the following methods are available for the mixture

critical constants:

constant: defines a constant critical temperature, critical pressure, critical specific volume, or acentric

factor for the mixture material.

mole-weighted-mixing-law: applies Equation . (p. ) for critical temperature, critical pressure,

critical specific volume, or acentric factor for the mixture material.

one-fluid-van-der-waals-mixing-law applies Equation . (p. ) and Equation . (p. ) for the

mixture critical temperature (depending on the real-gas model), Equation . (p. ) for the mixture

critical pressure, and Equation . (p. ) for the mixture molar volume.

Important

Ensure to click the Change/Create button so that all the above mentioned properties are

uploaded and are visible in the interface.

If you have selected mixing-law for the mixture ideal specific heat you will also need to enter

the ideal specific heat values for the individual mixture components. If you have not selected

constant as the option for any of the critical properties, you must enter the corresponding

pure component critical properties for the mixture components.

If the operating conditions in your model are in the subcritical regime, select Vapor or Liquid as

the Real Gas State in the Operating Conditions dialog box (Figure . : The Operating Conditions

for a Real Gas State (p. )). Alternatively, you can use the define/operating-condi-

tions/set-state text command. Note that the default is Vapor and therefore Vapor is assumed

if no changes are made to the Real Gas State settings. If the operating conditions in your model

are entirely in the supercritical regime, this setting will have no effect.

Figure . : The Operating Conditions for a Real Gas State

In addition, you may specify the state for a specific fluid zone or a specific phase (if you are using

multiphase modeling) by typing the following text command at the ANSYS Fluent console prompt:

> define boundary-conditions modify-zones change-zone-state

Select a name/id from fluid zones list [(liquid-zone fluid-)] liquid-zone

Set zone real-gas state:

:use global setting

:liquid

:vapor

[-]

:liquid

:vapor

[-]

..... Solution Strategies and Considerations for Cubic Equations of State Real Gas

Models

The flow modeling of real-gas flow is more complex and challenging than simple ideal-gas flow.

Therefore, the solution might converge at a slower rate with real-gas flow than when running ideal-

gas flow. It is recommended that you first attempt to converge your solution using first-order dis-

cretization then switch to second-order discretizations and re-iterate to convergence.

Special considerations apply if the operating regime in your model is fully or partly subcritical, where

the physical state may be vapor, liquid, or a vapor/liquid mixture. In the cubic EOS real-gas model,

the phase state is determined by the selection of the cubic root to calculate the molar-volume. This

is illustrated in Figure . : The PV Diagram for the Cubic Equation of State Real Gas Model (p. ),

which shows a pressure versus molar volume (PV) diagram, with a subcritical isotherm ABFED at

temperature T calculated from a cubic EOS. Curve C1CC2 represents the critical isotherm and curve

ACD the saturation dome. Points A, F, and D represent the three roots of the EOS at the saturation

pressure Ps, where A corresponds to the molar volume of saturated liquid, D to the molar volume

of saturated vapor and point F does not have a physical significance. Points A1 and D1 correspond

to the liquid and vapor molar volumes at pressure P1, which is lower than the saturation pressure.

The liquid and vapor molar volumes at pressure P2, which is higher than the saturation pressure,

are marked as A2 and D2 respectively. Points B and E, where the partial derivatives of pressure with

respect to volume

are , are called spinodal points. The loci of these points for all subcrit-

ical temperatures, the spinodal curve, is shown with the dashed curve BCE and sets the boundary

beyond which the equation of state is no longer valid, because the local derivative of pressure with

respect to volume becomes positive. State points inside the dome, up to the spinodal curve, are

called “metastable” because normally they only exist temporarily in small local regions until phase

change occurs.

Figure . : The PV Diagram for the Cubic Equation of State Real Gas Model

It is important to realize that the current implementation of the cubic equations of state real gas

model does not determine the saturation conditions and does not model the two-phase flow where

liquid and vapor coexist. In the subcritical regime and for conditions where the cubic EOS has three

roots, the phase state selection is controlled by your input of Vapor or Liquid for Real Gas State

in the Operating Conditions dialog box (Figure . : The Operating Conditions for a Real Gas

State (p. )). The default setting is Vapor, which corresponds to the state points to the right of the

vapor spinodal. With reference to Figure . : The PV Diagram for the Cubic Equation of State Real

Gas Model (p. ), for the operating point at temperature T and pressure P1, if the Real Gas State

is set to Vapor, the molar volume at point D1, which corresponds to superheated vapor, will be se-

lected in the calculation. On the other hand, if you have selected Liquid, the molar volume of point

A1 will be taken, and the corresponding state will be metastable superheated liquid. Similarly for

pressure P2, which is higher than the saturation pressure Ps, if you select Liquid for Real Gas State,

the liquid molar volume at A2 will be computed, and if you select Vapor the molar volume will

correspond to the subcooled vapor state point D2.

In case the calculations fall inside the saturation dome, the solver will not limit the solution, but if

conditions are predicted that extend beyond the vapor spinodal curve a warning will be issued:

temperature is below the spinodal point in  cells on zone .

Cubic equations of state real gas models are not available for two-phase flows but can be applied

to conditions of supercritical pressure

and subcritical temperature

, where the fluid is in

the liquid state, and the supercritical liquid co-exists with gas and supercritical fluid in the same

simulation. In those cases, phase change may take place, without any of the flow conditions falling

inside the saturation dome.

For multicomponent simulations, when Diffusion Energy Source is enabled in the Species Model

dialog box, the species energy diffusion is by default suppressed in the supercritical liquid regime

and across the gas-liquid boundary. The diffusion energy source can be included in the liquid regime

using the define/models/species/liquid-energy-diffusion? text command.

..... Using the Cubic Equation of State Models with the Lagrangian Dispersed

Phase Models

If your simulation contains a liquid stream, the appropriate modeling approach in the various oper-

ating condition regimes is as follows:

. For

a liquid phase does not exist.

. In the region

, you can define the flow streams directly in the boundary conditions by setting the

appropriate pressure and temperature and the properties will be computed directly by the cubic EOS.

. For

or

, a stream can exist in liquid phase when its temperature

. If you would like to

model phase change in this regime, the following recommendations apply:

The DPM droplet and multicomponent models are adequate and recommended for the conditions

away from the critical point.This regime can be defined as

, where the liquid physical

properties can be assumed independent of pressure.

The region

is characterized by near-critical-point phenomena, such as strong liquid

density and specific heat dependence on both temperature and pressure.The DPM model can also

be used in this regime, but you should be cautious, as it will not take into consideration the near-

critical-point behavior. In addition, the applicability of the evaporation and boiling rate equations is

questionable in this regime.

If the pressure in your model is above the critical point, it is recommended to use the compressible-

liquid method for Density of the droplet material.

The temperature

gives an indication of the maximum droplet temperature for applicab-

ility of the DPM models for each droplet material. These temperature limits are listed in

Table . : Temperature Limits for Droplet Materials in ANSYS Fluent Database prodb.scm (p. ) for

many of the droplet materials in ANSYS Fluent's propdb.scm materials database. For supercritical

pressures (

), the DPM models can still be used provided the droplet temperatures remain below

the limit

.

Table . : Temperature Limits for Droplet Materials in ANSYS Fluent Database prodb.scm

Tlim (K)

Normal BP (K)

Pc (MPa)

Tc (K)

Material

.

.

.

.

Argon

.

.

.

.

Benzene

.

.

.

.

Helium

.

.

.

.

Hydrogen

.

.

.

.

Methyl-alcohol

.

.

.

.

Heptanes

.

.

.

.

Hexane

.

.

.

.

Octane

.

.

.

.

Pentane

.

.

.

.

Nitrogen

.

.

.

.

Oxygen

.

.

.

.

Toluene

.

.

.

.

Water

For high pressure simulations the boiling point will be different from the normal boiling point, and

for varying pressure applications the boiling point will vary with the droplet location in the domain.

When a cubic equation of state real gas model is enabled in a simulation that includes evaporating

droplet particles, the boiling point is calculated from the vapor pressure data directly, as the temper-

ature where the saturation vapor pressure equals the domain pressure. In addition, the latent heat

of the evaporating or boiling droplet will vary with the droplet temperature.

The latent heat at temperature

is given by

(.)

where

is the normal boiling point and

is the latent heat at the normal boiling point.

In the Create/Edit Materials dialog box you must enter the Normal Boiling Point (NBP) and the

(.)

where

Latent Heat at NBP for the droplet-particle Material Type. These inputs will be used for calculating

the Latent Heat at the reference temperature (see Equation .) and the latent heat in the droplet

energy balance during vaporization and boiling according to Equation . (p. ).

Important

The constant property option is disabled for the Saturation Vapor Pressure property

when a real gas model is used in the simulation. Also, ensure to enter the appropriate

droplet saturation vapor pressure data to cover the complete pressure/temperature

range in your model.

Finally when a cubic equation of state real-gas model is enabled in a simulation with droplet models,

the condition for switching from the vaporization to the boiling law will be

(.)

where

is the saturation vapor pressure and P is the domain pressure. If

while in the

boiling law, the model will switch back to the vaporization law. Under supercritical pressure conditions

(

), the vaporization models are applicable at droplet temperatures below the critical point, and

the switching condition from vaporization to boiling

is never met because the vapor pressure

curve is defined only up to the critical point.

For the multicomponent droplets in the supercritical pressure regime, failure of the saturation tem-

perature calculation algorithm may indicate that the droplet has approached the critical temperature,

provided that you have entered accurate vapor pressure data for all components. In such a case,

you can use the following text command:

define/models/dpm/options/treat-multicomponent-saturation-temperature-

failure?

Dump multicomponent particle mass if the saturation temperature calcu-

lation fails? [no] y

When this option is enabled, ANSYS Fluent dumps the particle mass into the continuous phase if

the saturation temperature calculation fails.

..... Postprocessing the Cubic Equations of State Real Gas Model

All postprocessing functions properly report and display the current thermodynamic and transport

properties of the selected real gas model. The thermodynamic and transport properties controlled

by the cubic equations of state real gas model include the following:

density

enthalpy

entropy

sound speed

specific heat

any quantities that are derived from the properties listed above (for example, total quantities, ratio of

specific heats)

In addition to the properties listed above, you can also report

compressibility factor

reduced temperature

reduced pressure

spinodal temperature

subcritical condition

If you are modeling a real-gas mixture you can report the composition-dependent mixture critical

properties

The NIST real gas models use the National Institute of Standards and Technology (NIST) Thermodynamic

and Transport Properties of Refrigerants and Refrigerant Mixtures Database Version . (REFPROP v9.)

to evaluate thermodynamic and transport properties of approximately  fluids or a mixture of these

fluids.

fluids.

The REFPROP v9. database is a shared library that is dynamically loaded into the solver when you

enable one of the NIST real gas models in an ANSYS Fluent session. Once the NIST real gas model is

activated, control of relevant property evaluations is relinquished to the REFPROP database. All post-

processing functions will properly report and display the current thermodynamic and transport prop-

erties of the real gas.

.... Limitations of the NIST Real Gas Models

The following limitations exist for the NIST real gas model:

When you are using the NIST real gas models, the NIST materials defined in your simulation will appear

in the Create/Edit Materials Dialog Box (p. ) either with the name real-gas-_name , where _name  is

the NIST material selected for the single species model, or with the name real-gas-mixture for the multiple

species model.The inputs for the properties calculated by the NIST functions are disabled.You can use

the Create/Edit Materials Dialog Box (p. ) to define or modify:

– Mass diffusivity property in the real-gas-mixture material if you are using the multiple-species NIST

real gas model (note that the kinetic-theory option is not available)

– Radiation properties if you are modeling radiation

– Properties of materials other than the NIST real-gas-mixture or real-gas-fluid materials

The NIST real gas model assumes that the fluid you will be using in your ANSYS Fluent computation is

superheated vapor, supercritical fluid, or liquid. Note that subcritical flow conditions, where vapor coexists

with liquid in two-phase flow, are not supported. In addition, all fluid zones must contain the real gas;

you cannot include a real gas and another fluid in the same problem.

Pressure-inlet, mass flow-inlet, and pressure-outlet are the only inflow and outflow boundaries available

The mixture flow does not permit chemical reactions with the NIST real gas model.

The multicomponent NIST real gas models cannot be used with any of the multiphase models.You can,

however, use a NIST material in single-component multiphase flows.The model is compatible with the

Lagrangian Dispersed Phase Models only for the massless and inert particle types.

You cannot modify material properties in the REFPROP database libraries, or add custom materials to the

NIST real gas model.

The Diffusion Energy Source

in the energy equation (see The Energy Equation in the

Theory Guide) is not included with the nist-multispecies-real-gas-models and the pressure-based solver.

....The REFPROP v9. Database

The NIST real gas model supports  fluids from the REFPROP database. These include pure fluids

(with the file extension .fld) and pseudo-fluids (with the file extension .ppf). The fluids that are

supported by REFPROP v9. and used in the NIST real gas model are listed in Table . : Fluids Supported

by REFPROP v9. (p. ) (the corresponding property file name appears in parentheses, where it does

not coincide with the fluid name).

The REFPROP v9. database employs accurate pure-fluid equations of state that are available from

NIST. These equations are based on three models:

modified Benedict-Webb-Rubin (MBWR) equation of state

Helmholtz-energy equation of state

extended corresponding states (ECS)

For a fluid that consists of a multispecies-mixture the thermodynamic properties are computed by

employing mixing-rules applied to the Helmholtz energy of the mixture components.

Important

The database does not include transport property models for the species marked with *

in Table . : Fluids Supported by REFPROP v9. (p. ). As a result the NIST real gas model

with those species can only be used for modeling inviscid flow.

Table . : Fluids Supported by REFPROP v9.

nitrogen

butene

nonane

propanone (acetone.fld)

Dodecafluoro--methylpentan--one (novec649.fld)

air

octane

ammonia

orthohydrogen (orthohyd.fld)*

argon

oxygen

benzene

,-dimethylbenzene (oxylene.fld)*

n-butane (butane.fld)

parahydrogen (parahyd.fld)

dodecane (c12.fld)

pentane

methylcyclohexane (c1cc6.fld)

propane

cis--butene (c2butene.fld)

propene (propylen.fld)

n-propylcyclohexane (c3cc6.fld)

propyne

decafluorobutane (c4f10.fld)

,-dimethylbenzene (pxylene.fld)*

dodecafluoro-pentane (c5f12.fld)

,,-trichloro-,,-trifluoro-ethane (r113.fld)

trifluoro-iodo-methane (cf3i.fld)

,-dichloro-,,,-tetrafluoro-ethane (r114.fld)

carbondioxide

chloro-pentafluoro-ethane (r115.fld)

carbonmonoxide

hexafluoro-ethane (r116.fld)

carbonoxidesulfide (cos.fld)*

trichloro-fluoro-methane (r11.fld)

cyclohexane (cyclohex.fld)

hexafluoro-propene (r1216.fld)

cyclopentane (cyclopen.fld)

chloro-,,-trifluoroprop--ene (r1233zd.fld)

cyclopropane (cyclopro.fld)

,,,-tetrafluoroprop--ene (r1234yf.fld)

deuterium (d2.fld)

trans-,,,-tetrafluoro-propene (r1234ze.fld)

deuteriumoxide (d2o.fld)

,-dichloro-,,-trifluoro-ethane (r123.fld)

octamethyl-cyclotetra-siloxane (d4.fld)

chloro-,,,-tetrafluoro-ethane (r124.fld)

decamethyl-cyclopentasiloxane(d5.fld)

pentafluoro-ethane (r125.fld)

dodecamethyl-cyclohexasiloxane (d6.fld)

dichloro-difluoro-methane (r12.fld)

decane

,,,-tetrafluoro-ethane (r134a.fld)

diethylether (dee.fld)*

chlorotrifluoro-methane (r13.fld)

dimethylestercarbonicacid (dmc.fld)

,-dichloro--fluoroethane (r141b.fld)

methoxymethane (dme.fld)

chloro-,-difluoro-ethane (r142b.fld)

phenylethane (ebenzene.fld)*

,,-trifluoroethane (r143a.fld)

ethane

tetrafluoromethane (r14.fld)

ethyl alcohol (ethanol.fld)

,-difluoroethane (r152a.fld)

ethene (ethylene.fld)

fluoroethane (r161.fld)

fluorine

octa-fluoro-propane (r218.fld)

hydrogen sulfide (h2s.fld)

dichloro-fluoro-methane (r21.fld)

hydrogen chloride (hcl.fld)*

,,,,,,-hepta-fluoro-propane (r227ea.fld)

helium

chloro-difluoro-methane (r22.fld)

heptane

,,,,,-hexafluoro-propane (r236ea.fld)

hexane

,,,,,-hexafluoro-propane (r236fa.fld)

hydrogen (normal)

trifluoro-methane (r23.fld)

methyl--propene (ibutene.fld)

,,,,-pentafluoro-propane (r245ca.fld)

methylpentane (ihexane.fld)

,,,,-pentafluoro-propane (r245fa.fld)

,,-trimethylpentane (ioctane.fld)

difluoro-methane (r32.fld)

methylbutane (ipentane.fld)

,,,,-pentafluoro-butane (r365mfc.fld)

methylpropane (isobutan.fld)

% R125/% R134a/% R143a (r404a.ppf)*

krypton

krypton

% R32/% R125/% R134a (r407c.ppf)*

decamethyl-tetrasiloxane (md2m.fld)

methyl chloride (r40.fld)*

dodecamethyl-pentasiloxane (md3m.fld)

% R32/% R125 (r410a.ppf)*

tetradecamethyl-hexasiloxane (md4m.fld)

fluoro-methane (r41.fld)

octamethyl-trisiloxane (mdm.fld)

% R125/% R143a (r507a.ppf)*

methane

octafluoro-cyclobutane (rc318.fld)

methanol

methyl trifluoro-methyl ether (re143a.fld)*

methyl (Z,Z)-,-octadecadienoate (mlinolea.fld)

methyl-pentafluoro-ethyl-ether (re245cb2.fld)

methyl (Z,Z,Z)-,,-octadecatrienoate (mlinolen.fld)

,,-trifluoroethyl-difluoromethyl-ether (re245fa2.fld)

hexamethyl-disiloxane (mm.fld)

methyl-heptafluoro-propyl-ether (re347mcc.fld)

methyl cis--octadecenoate (moleate.fld)

sulfur hexafluoride (sf6.fld)

methyl hexadecanoate (mpalmita.fld)

sulfur dioxide (so2.fld)

methyl octadecanoate (mstearat.fld)

trans--butene (t2butene.fld)

,-dimethylbenzene (mxylene.fld)

methylbenzene (toluene.fld)

dinitrogen monoxide (n2o.fld)

water

neon

xenon

,-dimethylpropane (neopentn.fld)

nitrogen trifluoride (nf3.fld)*

.... Using the NIST Real Gas Models

When you enable one of the NIST real gas models (pure fluid or multiple-species mixture) and select

a valid material, ANSYS Fluent’s functionality remains the same as when you model fluid flow and

heat transfer using an ideal gas, with the exception of the Create/Edit Materials Dialog Box (p. ).

..... Activating the NIST Real Gas Model

Activating one of the NIST real gas models is a two-step process. First you enable either the single-

or multi-species NIST real gas model, and then you select the fluid material from the REFPROP

database.

. Enable the appropriate NIST real gas model by typing the following text command at the ANSYS Flu-

ent console prompt:

Pure fluid real gas model:

> define/user-defined/real-gas-models/nist-real-gas-model

use NIST real gas? [no] yes

Multi-species real gas model:

> define/user-defined/real-gas-models/nist-multispecies-real-gas-model

use multispecies NIST real gas? [no] yes

The list of available pure fluid materials you can select from will be displayed.

. Select material from the REFPROP database list:

Enter the name of a single pure fluid that you want to investigate as follows:

select real-gas data file [""]  methane.fld

Enter the number of desired species in the mixture:

Number of species []

followed by the name of each fluid in quotation marks selected from the list printed in the

console:

select real-gas data file [""] nitrogen.fld

select real-gas data file [""] co2.fld

select real-gas data file [""] methane.fld

a.

Upon selection of a valid pure or multi-species fluids, ANSYS Fluent will load the relevant material

data from a library of pure fluids supported by the REFPROP database, and report that it is opening

the shared library (librealgas.so) where the compiled REFPROP database source code is

located. A list of properties for the specified material, including its applicable pressure and tem-

perature ranges, will also be reported in the console.

Important

Important

– For mixture flows, not all combinations of species mixtures are allowed.This could be

due to lack of data for one or more binary pairs. In such situations an error message

generated by NIST will be returned and displayed on the ANSYS Fluent console, and no

real gas material is allowed to be created. In some combinations the mixing data will

be estimated, a warning message will be displayed on the ANSYS Fluent console and

the mixture material allowed to be created.

– Transport property calculations are not supported for mixtures that include water with

molar concentration over %. If this limit is exceeded in your calculation, ANSYS Fluent

will issue a warning message.Transport equations are not available for the ammonia/wa-

ter mixture and for mixtures with alcohols. As a result, the NIST real gas model with

those mixtures can only be used for modeling inviscid flow.

. If you want to use NIST lookup tables in your simulation, you can create them as described in the fol-

lowing sections:

Creating Full NIST Look-up Tables  (p. ) (single and multi-species materials with thermal properties

as well as saturation data for a fixed multi-species composition)

Creating Binary Mixture Saturation Tables for Binary Mixtures (p. ) (binary mixtures only)

. (cases with no NIST tables only) If you would like to model flow in the liquid state, you can use the set-

state TUI command. Note that the default state is vapor, so if you do not go through this step, vapor

is assumed. Also, if the flow conditions do not permit liquid to exist, a vapor calculation will be performed

instead.

instead.

> define/user-defined/real-gas-models/set-state

Select vapor state (else liquid)? [yes]

the multiphase model) by typing the following text command at the ANSYS Fluent console

prompt:

:liquid

:vapor

[-]

..... Creating Full NIST Look-up Tables

By default, the NIST functions are called directly each time the thermal properties are updated during

iteration. Alternatively, you can use the NIST look-up tables in your simulation as described below.

Computing the look-up table offers two advantages:

Reduction in computation time because the NIST functions do not need to be called each time the

thermal properties are updated

The look-up table created is applicable to both liquid and vapor phases

To create a full NIST look-up table, first enable the NIST real gas model as described in Activating

the NIST Real Gas Model (p. ), and then follow these steps:

. When prompted with Create Full NIST LookUp Tables for multi components? [no],

answer yes.

. Specify parameters for the look-up table generation.

For both single- and multi-species real gas models, you need to specify:

Pressure and temperature bounds for the table

You must ensure that the temperature and pressure bounds you specify are strictly within the

stated limits of applicability that are displayed when the NIST model is loaded.

Number of pressure, temperature, and saturation points, which determines the resolution of the

property look-up table

The minimum number of pressure and temperature points is  and there is no upper limit.

However, the larger the table, the greater the memory and computing time requirements. Use

a few test runs to strike the best balance of costs (memory and computing time) and accuracy.

For multi-species, you will also need to specify:

Upper and lower molar density bounds for bubble and dew point calculations

Molar density is used to build the saturation table. The default values work well for most

compositions.

The mixture composition on a mass or mole basis

You must ensure that the sum of all constituent fractions adds up to  when specifying

mass/molar fractions for the components. The maximum number of species is .

The bubble points and dew points filenames and the directory where you want to store the files.

Examples of inputs for the NIST look-up tables:

Min Pressure Value For NIST Table (pa) []

Max Pressure Value For NIST Table (pa) []

Min Temperature Value For NIST Table (k) [.]

Max Temperature Value For NIST Table (k) []

Number of Pressure Points For NIST Table []

Number of Temperature Points For NIST Table []

Number of Saturation Points For Bubble/Dew Curve []

NIST table created! Properties for both liquid and vapor phases included!

Tcrit = .391730e+ pcrit = .617700e+ Dcrit = .735823e+ Ttrp = .725200e+

Min Temperature Value For NIST Table (k) []

Please Select Mass Fractions [Y] or Molar Fractions [N] for Composition of Fluid

[yes]

Composition of Fluid will be set in Mass Fractions!

co2.fld [.]

methane.fld [.] .

Create NIST Saturation Curves for the same multi components?

[no] y

Min Molar Density For Bubble and Dew Points Calculations (mol/l) [.]

Max Molar Density For Bubble and Dew Points Calculations (mol/l) []

Bubble Points File Name ["Bubble_PT.xy"]

Dew Points File Name ["Dew_PT.xy"]

Directory to store Saturation Files [""]

Start NIST Look-Up Table Calculations ...

Property Table... . percent completed!

NIST table for -components created! Properties for both liquid and vapor phases included!

End NIST Look-Up Table Calculations

Use the created NIST Lookup Table for thermal property calculations? [no] y

Once the table is created, you must confirm that you want to use the look-up table for thermal

properties calculations when prompted.

Use the created NIST Lookup Table for thermal property calculations? [no] yes

The created NIST Lookup Table will be used to calculate the thermal properties!

If properties are needed at conditions outside the limits you have specified for the table, Fluent

will automatically call the original NIST model functions to calculate the thermal properties. If

more than % of the property evaluations require computation outside the look-up table, Fluent

will print a message indicating the percentage of calculations using direct computation. This can

be used as an indicator to adjust the temperature and pressure ranges for the table to minimize

the computational cost.

For multi-species real gas properties, the following tables will be created:

fluid properties

saturation conditions

Remarks and Limitations on Using Multi-Species Full NIST look-up Tables

The look-up table is not saved with the case file. If you restart Fluent or re-read case and data files into

the current Fluent session, the table will be cleared and you must go through the steps above to re-create

it before running a simulation.

For computation of saturation properties for the bubble and dew points for a single- or multiple-species,

Fluent provides macros that you can use in UDFs. See NIST Real Gas Saturation Properties in the Fluent

Customization Manual for more information.

The tables apply for compressible fluids with material properties that are a function of local pressure and

temperature.The material properties covered by the table include fluids in the liquid and vapor phases.

The flashing applications between liquid and vapor phases can be conducted using saturation conditions

established for the fluid(s) using mass transfer models.

The property look-up tables and saturation tables are created for fixed fluid compositions.This means

the look-up tables are based on the following assumptions:

– Mixture composition is constant

– No chemical reactions are involved

– No mixing of fluids of different compositions, including no mixing between phases

The look-up table only applies to single-species/multi-species in single-phase flows.

The temperature and pressure bounds must be specified within the stated limits of applicability that are

displayed when the NIST model is loaded.

When specifying the table size, it is important to pick temperature and pressure ranges that are large

enough to satisfy the current flow conditions.

If the temperature and pressure ranges you specify are too narrow, Fluent uses the NIST model to calculate

the thermal properties.The time saved by creating the table will be negated if the percentage of calcu-

lations performed outside of the table is greater than %.This percentage is printed, so you can use it

as an indicator for adjusting the temperature and pressure range of the table.

For multi-species table, the bubble and dew points are saved into files(Fluent plot file format) called

Bubble_PT.xy and Dew_PT.xy in the working directory.

The look-up table is a structured table and may not be suitable for simulating flow behaviors near the

critical point when higher resolution is required.

..... Creating Binary Mixture Saturation Tables for Binary Mixtures

To create a saturation data look-up table for binary species mixtures (mixtures of two species only),

first enable the NIST real gas model as described in Activating the NIST Real Gas Model (p. ) and

then follow these steps:

answer no.

. When prompted with Create Saturation Table For Binary Mixture Only? [no],

answer no.

Important

Not all binary mixtures can be computed from the Fluent built-in NIST model. The al-

lowed combination of materials is determined by the current database of NIST that

can be found in hmx.bnc in the ANSYS Fluent installation directory.

. Specify parameters for the binary saturation data look-up table generation:

The number of saturation curves

The number of points for each saturation curve

The default number is . The actual number of points for each bubble and dew curve may

be different than specified because the NIST model may not yield valid computation results

for every density point for a given mass fraction.

The molar density is used to build the saturation table. You should provide reasonable values

for the minimum and maximum molar densities corresponding to gas phase at low pressure

and high temperature, and liquid phase at high pressure and low temperature. The default

values (as shown in the example below) are a good starting point. You may need to adjust

these values if there is not enough data in the selected range.

The filenames for bubble points and dew points and the existing directory where you want to store

the files.

An example of inputs for the NIST binary look-up table:

Number of Mass Fraction Points For Binary Mixture []

Directory to store Saturation Files [""] out

The lookup table builds multiple sets of the bubble and dew points for the binary mixture with

mass fractions for the first component between  and . The second component mass fraction

is equal to the first component mass fraction subtracted from unity. The number of saturation

curves is determined by the number of mass fraction points that you specified.

Once the lookup table is created, Fluent saves the bubble and dew points data into files and

directory you specified.

NIST Binary Saturation Files

NIST binary saturation files store saturation data lookup table for bubble and dew points for a binary

mixture with mass fractions between  and . They can be used for mass and heat transfer modeling

involving phase changes.

The binary saturation file structure is as follows. The file contains several data sets for bubble/dew

point curves for a series of mass fractions. Each data set consists of the following three parts:

. Line :The mass fraction of the first species (a single float number between  and ).

. Line :The number of data pairs for saturation pressure and temperature.

. The specified number of lines that follow line : Data pairs of saturation pressure and temperature.The

last pressure-temperature pair corresponds to the critical condition.

The example below shows the saturation dew point data for the first two curves, both with

pressure-temperature pairs. The first data set is for  and the second is for a . mass fraction

of the first species. The pressure-temperature critical condition is (.872200e+, .053220e+) for

the first curve and (.547305e+, .947561e+) for the second curve.

.

.142108e+ .036800e+

.314020e+ .099093e+

.202771e+ .294505e+

.833626e+ .489918e+

.890130e+ .685331e+

.219542e+ .880744e+

.025174e+ .076156e+

.354397e+ .271569e+

.182515e+ .466982e+

.011733e+ .662395e+

.201942e+ .857807e+

.872200e+ .053220e+

.

.509489e+ .891238e+

.257388e+ .428513e+

.252097e+ .631615e+

.090473e+ .752623e+

.775539e+ .831498e+

.318958e+ .883822e+

.735586e+ .917723e+

.042345e+ .938262e+

.258091e+ .949048e+

.402834e+ .952901e+

.495209e+ .951982e+

.547305e+ .947561e+

.....

.....

..... Changing the REFPROP Library and Fluid Files

In ANSYS Fluent, you can change the REFPROP library and the fluid files that are accessed by the

NIST real-gas model by entering the following text command in the ANSYS Fluent console:

/define/user-defined/real-gas-models/nist-settings

When prompted with

User-defined refprop library and fluids files?

The default names for the refprop library and the fluid file paths correspond to the REFPROP v9.

files provided with your ANSYS Fluent installation. You can revert to the older REFPROP v7..

database by accepting the default refprop library path and entering the following names at the

prompts for library name and fluid files path:

Select refprop library path ["path\fluent19..\realgas"]

Select refprop library name[“librealgas”] “librealgas7”

Select refprop fluid files path ["path\fluent19..\realgas\lib"] “path\fluent19..\realgas\lib7.”

where path is the ANSYS Fluent installation directory (for example, C:\Program Files\ANSYS

Inc\v195\fluent).

ANSYS Fluent will open REFPROP v7. library and report the information in the console.

To switch back to the default REFPROP v9. property database, enter the /define/user-

defined/real-gas-models/nist-settings command again and enter no at the prompt.

ANSYS Fluent will report the change in the console window.

.... Solution Strategies and Considerations for NIST Real Gas Model Simulation

The flow modeling of NIST real-gas flow is much more complex and challenging than simple ideal-

gas flow. Therefore, you should expect the solution to converge at much slower rate with real-gas

flow than when running ideal-gas flow. Also due to the complexity of the equations used in property

evaluations, converging a solution with the real-gas model is in general done at much lower Courant

values when you are using the density-based solver, or at much lower under-relaxation values if you

are using the pressure-based solver. It is recommended that you first attempt to converge your

solution using first-order discretization, then switch to second-order discretizations and re-iterate to

convergence.

The real-gas properties in NIST are defined within a limited/bounded range. It is important that the

flow conditions you are prescribing fall within the range of the database. It is possible that you specify

flow at a state that is physically valid but otherwise not defined in the database. In this situation the

solution will diverge or immediately generate an error message on the ANSYS Fluent console as soon

as the state crosses the limit of the database. In some instances, the actual converged state is just

within the bounded defined database but only transitory outside the range. In this situation the di-

vergence can be avoided by lowering the Courant value or under-relaxation factors so a less aggressive

convergence rate is adapted.

Finally, if you attempt to initialize the flow from an inlet flow conditions and an error message is

generated from one of the property routines, then this is an indicator that the flow conditions you

have specified is not defined within the range of the database.

.....Writing Your Case File

When you save your completed real gas model to a case file, the linkage to the shared library con-

taining real gas properties will be saved to the case file (along with property data for the material

you selected in the NIST real gas model). Consequently, whenever you read your case file in a later

session, ANSYS Fluent will load and report this information to the console during the read process.

..... Postprocessing

by the NIST real gas model include the following:

density

enthalpy

entropy

molecular viscosity

density

enthalpy

entropy

thermal conductivity In addition to the properties listed above, you can also report

The user-defined real gas model (UDRGM) has been developed to allow you to write your own custom

real gas model to fit your particular modeling needs. It also allows you to simulate a single-species

flow, multiple-species mixture flow, multiphase flow, or volumetric reactions.

The following limitations exist for the UDRGM:

.... Limitations of the User-Defined Real Gas Model

You cannot include more than one user-defined real gas material (fluid or mixture) in the same problem.

However, you can use other materials together with real gas in your simulation.

When you are using the UDRGM, the materials defined in your real gas UDF will appear in the Create/Edit

Materials Dialog Box (p. ) with the name real-gas-fluid or real-gas-mixture and all physical and ther-

modynamic property inputs disabled. Use the Create/Edit Materials Dialog Box (p. ) to define or modify:

– Mass diffusivity property in the real-gas-mixture material if you are modeling multicomponent flow.

– Chemical reactions in the real-gas-mixture if you are modeling reacting flow.

– Radiation properties for the real-gas-mixture or the real-gas-fluid materials if you are modeling radiation.

– Properties of materials other than the user-defined real-gas-mixture or real-gas-fluid materials.

Note

Note

If you are using the UDRGM together with other materials from ANSYS Fluent's property

database in dispersed phase or multiphase calculations, take care to use the same refer-

ence temperature as in ANSYS Fluent in your real-gas UDF. The reference temperature

in ANSYS Fluent is . K.

The UDRGM can be used with the Eulerian multiphase models.

The UDRGM is compatible with the Lagrangian Dispersed Phase Models. Refer to Using the Cubic Equation

of State Models with the Lagrangian Dispersed Phase Models (p. ) for guidelines and restrictions of this

approach.

The real gas models cannot be used with the non-premixed, partially premixed, and composition PDF

transport combustion models. Chemical reactions can however be modeled with the finite rate and eddy

dissipation models. Note that the Dimension Reduction model is not available with the real gas models.

The UDRGM requires a library of functions written in the C programming language. Moreover, there

are certain coding requirements that need to be followed when writing these functions. Sample real

gas function libraries are provided to assist you in writing your own UDRGM. When UDRGM functions

are compiled, they will be grouped in a shared library that later will be loaded and linked with the

ANSYS Fluent executable. The procedure for using the UDRGM is defined as follows:

. Define the real gas equation of state and all related thermodynamic and transport property equations.

. Create a C source code file that conforms to the format defined in this section.

. Start ANSYS Fluent and set up your case file in the usual way.

. Compile your UDRGM C library and build a shared library file (you can use the available compiled UDF

utilities in either the graphical user interface or the text command interface).

. Load your newly created UDRGM library via the text command menu:

If a single-species UDRGM to be used, then the text command menu is:

> define/user-defined/real-gas-models/user-defined-real-gas-model

use user defined real gas? [no] yes

On the other hand, if you are simulating multiple-species UDRGM flow, then the text command

menu to use is:

> define/user-defined/real-gas-models/user-defined-multispecies-real-gas-model

use user multispecies defined real gas? [no] yes

Upon activating the UDRGM, the function library will now supply the fluid material properties for

your case.

. You can simulate volumetric reactions with your real gas model using the Species Model Dialog Box (p. ),

or the text interface (define/models/species/volumetric-reactions? ).

You can access the Species Model from the tree by going to Setup/Models/Species and double-

clicking Species.

In the Species Model Dialog Box (p. )

Enable Species Transport under Model.

Enable Volumetric under Reactions.

Select the appropriate Turbulence-Chemistry Interaction option.

Set up the reaction by clicking the Edit... button for the real-gas-mixture Mixture Material.

Important

Important

Note that the fluid materials and their properties, appearing in the Create/Edit Ma-

terials Dialog Box (p. ), are the ones defined in your real gas UDF. You cannot

modify the materials via this dialog box, however, you can set up the volumetric re-

action. If you would like to modify the mixture materials and their properties, this

should be done in the real gas UDF. The volumetric reactions for your real gas mixture

are defined in the same way as for any ANSYS Fluent mixture. For details, refer to

Defining Reactions (p. ).

Alternatively, the chemical reactions can be set up using the define/models/species and

define/materials text command.

Important

Note that the chemical reactions should be activated after your real gas UDF has been

built and loaded. It is also recommended to test and validate your real gas UDF, running

the cold flow calculation prior to attempting to solve the reacting flow. Also, make sure

that the applicability range of the real gas functions in your UDF fully covers the tem-

perature and pressure range of the reacting flow calculation.

. Run your calculation.

When using the UDRGM the robustness of the solver and the speed of flow convergence will largely

depend on the complexity of the material properties you have defined in your UDF. It is important

to understand the operational range of the property functions you are coding so you can simulate

the flow within that range.

....Writing the UDRGM C Function Library

Creating a UDRGM C function library is reasonably straightforward; however, your code must make

use of specific function names and macros, which will be described in detail below. The basic library

requirements are as follows:

The code must contain the udf.h file inclusion directive at the beginning of the source code.This allows

the definitions for DEFINE macros and other ANSYS Fluent functions to be accessible during the compil-

ation process.

The code must include at least one of the UDF’s DEFINE functions (that is DEFINE_ON_DEMAND) to be

able to use the compiled UDFs utility (see the sample UDRGM codes provided below).

Any values that are passed to the solver by the UDRGM or returned by the solver to the UDRGM are assumed

to be in SI units.

You must use the principal set of functions listed below in your UDRGM library.These functions are the

mechanism by which your thermodynamic property data are transferred to the ANSYS Fluent solver. Note

that ANYNAME can be any string of alphanumeric characters, and allows you to provide unique names to

your library functions.

Function inputs from the ANSYS Fluent solver consist of one or more of the following variables:

= Temperature, K

= Pressure, Pa

= Density, kg/

[] = Species mass fraction

cell = Cell or face index, depending on whether the thread is a cell or face zone; NULL_CELL

is passed when the function is called without a cell/face context

thread = Pointer to thread structure; NULL is passed when the function called without thread

context

Important

[]: ANSYS Fluent solver returns a value of . for

[] in single-species flows. For multiple-

species flows,

context

Important

[] is a vector array containing species mass fraction in an order defined by the

user setup function.

For temperature, density, pressure and species mass fractions the UDRGM code should use the

values provided as functions arguments.The corresponding values in the solution arrays, which

are accessible via cell index and thread pointer, may temporarily differ from these depending

on algorithmic details, and the function arguments take precedence.

The UDRGM function names and argument lists, followed by a short description of the function, are

void ANYNAME_Setup(Domain *domain, cxboolean vapor_phase, char *species_list,

int (*messagefunc)(const char *format,...), void (*errorfunc)(const char

format, ...))

performs model setup and initialization. Can be used to read data and parameters related to your UDRGM.

When writing UDFs for multiple-species, use this function to specify the number of species and the name

of the species as shown in the multiple-species example.The Boolean variable, vapor_phase, passes

to your UDF the setting of the text-interface command define/user-defined/real-gas-mod-

els/set-state.

The messagefunc argument is a function that you can use for including diagnostic output in

the transcript file, and the errorfunc argument is the equivalent of error reporting. The format

string and additional arguments follow the same syntax as the printf C function.

double ANYNAME_density(cell_t cell, Thread *thread, cxboolean vapor_phase,

double T, double P, double yi[])

returns the value of density as a function of phase, temperature, pressure and species mass-fraction if

applicable.The Boolean variable vapor_phase passes to your UDF the setting of the text-interface

command define/user-defined/real-gas-models/set-state, or, if applicable, the zone

state set by the text-interface command define/boundary-conditions/modify-

zones/change-zone-state.

Important

Since this function is called numerous times during each solver iteration, it is important

to make this function as numerically efficient as possible.

double ANYNAME_specific_heat(cell_t cell, Thread *thread, double T, double

Rho, double P, double yi[])

returns the real gas specific heat at constant pressure as a function of temperature, density, absolute

pressure, and species mass-fraction if applicable.

double ANYNAME_enthalpy(cell_t cell, Thread *thread, double T, double Rho,

double P, double yi[])

returns the enthalpy as a function of temperature, density, absolute pressure, and species mass-fraction

if applicable.

double ANYNAME_entropy(cell_t cell, Thread *thread, double T, double Rho,

returns the entropy as a function of temperature, density, absolute pressure, and species mass-fraction

double ANYNAME_mw(double yi[])

returns the fluid molecular weight.

double ANYNAME_speed_of_sound(cell_t cell, Thread *thread, double T, double

returns the value of speed of sound as a function of temperature, density, absolute pressure, and species

mass-fraction if applicable.

double ANYNAME_viscosity(cell_t cell, Thread *thread, double T, double Rho,

returns the value of dynamic viscosity as a function of temperature, density, absolute pressure, and

species mass-fraction if applicable.

double ANYNAME_thermal_conductivity(cell_t cell, Thread *thread, double T,

double Rho, double P, double yi[])

returns the value of thermal conductivity as a function of temperature, density, absolute pressure, and

double ANYNAME_rho_t(cell_t cell, Thread *thread, double T, double Rho,

returns the value of

at constant pressure as a function of temperature, density, absolute pressure,

and species mass-fraction if applicable.

double ANYNAME_rho_p(cell_t cell, Thread *thread, double T, double Rho,

at constant temperature as a function of temperature, density, absolute pressure,

double ANYNAME_enthalpy_t(cell_t cell, Thread *thread, double T, double

and species mass-fraction if applicable. Note that by definition

, so this function should

simply return the specific heat value.

double ANYNAME_enthalpy_p(cell_t cell, Thread *thread, double T, double

double ANYNAME_enthalpy_prime (cell_t cell, Thread *thread, double T, double

Rho, double P, double yi[], double hi[])

returns the value of the mixture enthalpy as a function of temperature, density, absolute pressure, and

species mass fraction. In addition, your UDF must set the elements of the double array hi[] to the en-

thalpy of each species, in the same order as they are referenced in the mass fraction array yi[]. Note

that the enthalpy in the function enthalpy_prime is defined as the sum of sensible enthalpy plus

species formation enthalpy, and you should make sure that its computation is consistent with the

sensible enthalpy function ANYNAME_enthalpy.The function ANYNAME_enthalpy_prime is required

for the calculation of the heat of reactions, if chemical reactions are being simulated. If you are not

solving reacting flows, the function ANYNAME_enthalpy_prime can simply be omitted.

At the end of the code you must define a structure of type RGAS_Function whose members are

pointers to the principal functions listed above. The structure is of type RGAS_Function and its

name is RealGasFunctionList.

Important

It is imperative that the sequence of function pointers shown below be followed. Otherwise,

your real gas model will not load properly into the ANSYS Fluent code.

UDF_EXPORT RGAS_Functions RealGasFunctionList =

{

ANYNAME_Setup,                   /* Setup initialize */

ANYNAME_density,                 /* density */

ANYNAME_enthalpy,                /* sensible enthalpy */

ANYNAME_entropy,                 /* entropy */

ANYNAME_specific_heat,           /* specific_heat */

ANYNAME_mw,                      /* molecular_weight */

ANYNAME_speed_of_sound,          /* speed_of_sound */

ANYNAME_viscosity,               /* viscosity */

ANYNAME_thermal_conductivity,    /* thermal_conductivity */

ANYNAME_rho_t,                   /* drho/dT |const p */

ANYNAME_rho_p,                   /* drho/dp |const T */

ANYNAME_enthalpy_t,              /* dh/dT |const p */

ANYNAME_enthalpy_p               /* dh/dp |const T */

ANYNAME_enthalpy_prime           /* enthalpy */

};

If volumetric reactions are not being simulated, then the function ANYNAME_enthalpy_prime can

be removed or ignored from the RealGasFunctionList structure described here.

The principal set of functions described are the only functions in the UDRGM that will be interacting

directly with the ANSYS Fluent code. In many cases, your model may require further functions that

will be called from the principal function set. For example, when multiple-species real gas model

UDFs are written, the principal functions will return the mixture thermodynamic properties based on

some specified mixing-law. Therefore, you may want to add further functions that will return the

thermodynamic properties for the individual species. These auxiliary functions will be called from the

principal set of functions. See User-Defined Real Gas Models (UDRGM) in the Fluent Customization

Manual for examples that clearly illustrate this strategy.

.... Compiling Your UDRGM C Functions and Building a Shared Library File

This section presents the steps you must follow to compile your UDRGM C code and build a shared

library file. This process requires the use of a C compiler. For more details on compiler requirements,

see Compilers in the Fluent Customization Manual. To use the UDRGM you must first build the UDRGM

library by compiling your UDRGM C code and then load the library into the ANSYS Fluent code. The

UDRGM shared library is built in the same way that the ANSYS Fluent executable itself is built. Internally,

a script called Makefile is used to invoke the system C compiler to build an object code library

that contains the native machine language translation of your higher-level C source code. This shared

library is then loaded into ANSYS Fluent (either at run time or automatically when a case file is read)

by a process called dynamic loading. The object libraries are specific to the computer architecture

being used, as well as to the particular version of the ANSYS Fluent executable being run. The libraries

must, therefore, be rebuilt any time ANSYS Fluent is upgraded, when the computer’s operating system

level changes, or when the job is run on a different type of computer. The general procedure for

compiling UDRGM C code is as follows:

Place the UDRGM C code in the folder, that is, where your case file resides.

Launch ANSYS Fluent.

Read your case file into ANSYS Fluent.

You can now compile your UDRGM C code and build a shared library file using either the graphical interface

or the text command interface.

Important

To build UDRGM library you will use the compiled UDF utilities. However, you will not use

the UDF utilities to load the library. A separate loading area for the UDRGM library will be

used.

..... Compiling the UDRGM Using the Graphical Interface

used.

If the build is successful, then the compiled library will be placed in the appropriate architecture

folder (for example, win64/2d). By default the library name is libudf.so (libudf.dll on

Windows).

More information on compiled UDFs and building libraries using the ANSYS Fluent graphical user

interface can be found in the Fluent Customization Manual.

..... Compiling the UDRGM Using the Text Interface

The UDRGM library can be compiled in the text command interface as follows:

Select the menu item define → user-defined → compiled-functions .

Select the compile option.

Enter the compiled UDF library name.

Important

The name given here is the name of the folder where the shared library (for example,

libudf) will reside. For example, if you press Enter then a folder should exist with

the name libudf, and this folder will contain a library file called libudf. If, however,

you type a new library name such as myrealgas, then a folder called myrealgas

will be created and it will contain the library libudf.

Continue on with the procedure when prompted.

Enter the C source file names.

Important

Ideally you should place all of your functions into a single file. However, you can split

them into separate files if desired.

Enter the header file names, if applicable. If you do not have an extra header file then press Enter when

prompted.

ANSYS Fluent will then start compiling the UDRGM C code and put it in the appropriate architecture

folder.

Example:

> define/user-defined/compiled-functions

load OR compile ? [load]  compile

Compiled UDF library name: ["libudf"] my_lib

folder.

Example:

Make sure that UDF source files are in the folder

that contains your case and data files. If you have

an existing libudf folder, please remove this

folder to ensure that latest files are used.

Continue? [yes] RETURN

Give C-Source file names:

First file name: [""] my_c_file.c RETURN

Next file name: [""] RETURN

Give header file names:

First file name: [""] my_header_file.h RETURN

..... Loading the UDRGM Shared Library File

Load the UDRGM library:

Go to the following menu item in the text command interface.

define → user-defined → real-gas-models

Select one of the following

– user-defined-real-gas-model if you are modeling a single-species real gas fluid

– user-defined-multispecies-real-gas-model if you are modeling a multiple-species fluid-

mixture

Turn on the real gas model.

– For single-species:

use user defined real gas? [no]   yes

– For multiple-species:

use multispecies user defined real gas? [no]   yes

ANSYS Fluent will ask for the location of the user-defined real gas library. You can enter either the

name of the folder where the UDRGM shared library is called or the entire path to the UDRGM

shared library.

If the loading of the UDRGM library is successful you will see a message similar to the following:

Opening user-defined realgas library "RealgasLibraryname"...

Library "RealgasDirName/lnamd64/2d/libudf.so" opened

Setting material "air" to a real-gas...

Loading Real-RealGasPrefexLable Library:

.... UDRGM Example: Ideal Gas Equation of State

This section describes an example of a user-defined real gas model. You can use this example as the

basis for your own UDRGM code. In this simple example, the standard ideal gas equation of state is

used in the UDRGM. See User-Defined Real Gas Models (UDRGM) in the Fluent Customization Manual for

more examples of UDRGM functions, including multi-species real gas and reacting real-gas examples.

= pressure

= temperature

= specific heat

= enthalpy

= entropy

= density

= speed of sound

= universal gas constant/molecular weight

The ideal gas equation of state can be written in terms of pressure and temperature as

(.)

The specific heat is defined to be constant

= ..

The enthalpy is, therefore, defined as

(.)

and entropy is given by

(.)

where

= . K and

=  Pa

The speed of sound is simply defined as

(.)

The density derivatives are:

(.)

(.)

The enthalpy derivatives are:

(.)

(.)

When you enable the real gas model and load the library successfully into ANSYS Fluent, you will be

using the equation of state and other fluid properties from this library rather than the one built into

the ANSYS Fluent code.

..... Ideal Gas UDRGM Code Listing

/**********************************************************************/

/* User Defined Real Gas Model :                                      */

/* For Ideal Gas Equation of State                                    */

/*                                                                    */

#include "udf.h"

#include "stdio.h"

#include "ctype.h"

#include "stdarg.h"

#define MW . /* molec. wt. for single gas (Kg/Kmol) */

#define RGAS (UNIVERSAL_GAS_CONSTANT/MW)

static int (*usersMessage)(const char *, ...);

static void (*usersError)(const char *, ...);

DEFINE_ON_DEMAND(I_do_nothing)

{

/* This is a dummy function to allow us to use */

/* the Compiled UDFs utility      */

}

void IDEAL_error(int err, char *f, char *msg)

{

if (err)

usersError("IDEAL_error (%d) from function: %s\n%s\n", err, f, msg);

}

void IDEAL_Setup(Domain *domain, cxboolean vapor_phase, char *filename,

int (*messagefunc)(const char *format, ...),

void (*errorfunc)(const char *format, ...))

{

/* Use this function for any initialization or model setups*/

usersMessage = messagefunc;

usersError  = errorfunc;

usersMessage("\nLoading Real-Ideal Library: %s\n", filename);

}

double IDEAL_density(cell_t cell, Thread *thread,

cxboolean vapor_phase, double Temp, double press, double yi[])

{

double r = press / (RGAS * Temp); /* Density at Temp & press */

return r;      /* (Kg/m^) */

}

double IDEAL_specific_heat(cell_t cell, Thread *thread,

double Temp, double density, double P, double yi[])

{

double cp = . ;

return cp;     /* (J/Kg/K) */

}

double IDEAL_enthalpy(cell_t cell, Thread *thread,

{

double h = Temp * IDEAL_specific_heat(cell, thread, Temp, density, P, yi);

return h;      /* (J/Kg) */

}

#define TDatum .

#define PDatum .01325e5

double IDEAL_entropy(cell_t cell, Thread *thread,

{

double s = IDEAL_specific_heat(cell, thread, Temp, density, P, yi) * log(fabs(Temp / TDatum)) +

RGAS * log(fabs(PDatum / P));

{

return s;      /* (J/Kg/K) */

}

double IDEAL_mw(double yi[])

{

return MW;     /* (Kg/Kmol) */

}

double IDEAL_speed_of_sound(cell_t cell, Thread *thread,

{

double cp = IDEAL_specific_heat(cell, thread, Temp, density, P, yi);

return sqrt(Temp * cp * RGAS / (cp - RGAS)); /* m/s */

}

double IDEAL_viscosity(cell_t cell, Thread *thread,

{

double mu = .7894e-;

return mu;     /* (Kg/m/s) */

}

double IDEAL_thermal_conductivity(cell_t cell, Thread *thread,

double Temp, double density, double P,

double yi[])

{

double ktc = . ;

return ktc;      /* W/m/K */

}

double IDEAL_rho_t(cell_t cell, Thread *thread,

{

/* derivative of rho wrt. Temp at constant p */

double rho_t = -density / Temp;

return rho_t;     /* (Kg/m^/K) */

}

double IDEAL_rho_p(cell_t cell, Thread *thread,

{

/* derivative of rho wrt. pressure at constant T */

double rho_p = . / (RGAS * Temp);

return rho_p;    /* (Kg/m^/Pa) */

}

double IDEAL_enthalpy_t(cell_t cell, Thread *thread,

{

/* derivative of enthalpy wrt. Temp at constant p */

return IDEAL_specific_heat(cell, thread, Temp, density, P, yi);

}

double IDEAL_enthalpy_p(cell_t cell, Thread *thread,

{

/* derivative of enthalpy wrt. pressure at constant T  */

}

{

/* general form dh/dp|T = (/rho)*[  + (T/rho)*drho/dT|p] */

/* but for ideal gas dh/dp =         */

return . ;

}

{

IDEAL_Setup,                   /* initialize */

IDEAL_density,                 /* density */

IDEAL_enthalpy,                /* enthalpy */

IDEAL_entropy,                 /* entropy */

IDEAL_specific_heat,           /* specific_heat */

IDEAL_mw,                      /* molecular_weight */

IDEAL_speed_of_sound,          /* speed_of_sound */

IDEAL_viscosity,               /* viscosity */

IDEAL_thermal_conductivity,    /* thermal_conductivity */

IDEAL_rho_t,                   /* drho/dT |const p */

IDEAL_rho_p,                   /* drho/dp |const T */

IDEAL_enthalpy_t,              /* dh/dT |const p  */

IDEAL_enthalpy_p               /* dh/dp |const T  */

};

/**************************************************************/

.... Additional UDRGM Examples

You can find the following additional UDRGM examples in the Fluent Customization Manual:

The Aungier Redlich Kwong equation of state for single component flow. See UDRGM Example: Redlich-

Kwong Equation of State in the Fluent Customization Manual for details.

A simple example of a multi-species real-gas model. See UDRGM Example: Multiple-Species Real Gas

Model in the Fluent Customization Manual for details.

A real gas model example with the Aungier Redlich Kwong equation of state, ideal gas mixing rules and

volumetric reactions. See UDRGM Example: Real Gas Model with Volumetric Reactions in the Fluent Cus-

tomization Manual for details.

Chapter : Modeling Basic Fluid Flow

This chapter describes the basic physical models that ANSYS Fluent provides for fluid flow and the

commands for defining and using them. Models for flows in moving zones (including sliding and dy-

namic meshes) are explained in Modeling Flows with Moving Reference Frames (p. ), models for

turbulence are described in Modeling Turbulence (p. ), and models for heat transfer (including radi-

ation) are presented in Modeling Heat Transfer (p. ). An overview of modeling species transport and

reacting flows is provided in Modeling Species Transport and Finite-Rate Chemistry (p. ), details about

models for species transport and reacting flows are described in   Modeling Species Transport and Finite-

Rate Chemistry (p. ) – Modeling a Composition PDF Transport Problem (p. ), and models for pol-

lutant formation are presented in Modeling Pollutant Formation (p. ). The discrete phase model is

described in Modeling Discrete Phase (p. ), general multiphase models are described in Modeling

Multiphase Flows (p. ), and the melting and solidification model is described in Modeling Solidification

and Melting (p. ). For information on modeling porous media, porous jumps, and lumped parameter

fans and radiators, see Cell Zone and Boundary Conditions (p. ).

The information in this chapter is presented in the following sections:

.. User-Defined Scalar (UDS) Transport Equations

.. Periodic Flows

.. Swirling and Rotating Flows

.. Compressible Flows

.. Inviscid Flows

... UDS Theory

... Setting Up UDS Equations in ANSYS Fluent

ANSYS Fluent can solve the transport equation for an arbitrary, user-defined scalar (UDS) in the same

way that it solves the transport equation for a scalar such as species mass fraction. Extra scalar transport

equations may be needed in certain types of combustion applications or for example in plasma-en-

hanced surface reaction modeling. ANSYS Fluent allows you to define additional scalar transport

equations in your model in the User-Defined Scalars Dialog Box (p. ).

UDS theory is described in the following sections:

.... Single Phase Flow

.... Multiphase Flow

For an arbitrary scalar

, ANSYS Fluent solves the equation

(.)

where

and

are the diffusion coefficient and source term supplied by you for each of the

scalar equations. Note that

is defined as a tensor in the case of anisotropic diffusivity. The diffusion

term is therefore

For isotropic diffusivity,

could be written as

where I is the identity matrix.

For the steady-state case, ANSYS Fluent will solve one of the three following equations, depending

on the method used to compute the convective flux:

If convective flux is not to be computed, ANSYS Fluent will solve the equation

(.)

where

and

scalar equations.

If convective flux is to be computed with mass flow rate, ANSYS Fluent will solve the equation

(.)

(.)

It is also possible to specify a user-defined function to be used in the computation of convective flux. In

this case, the user-defined mass flux is assumed to be of the form

(.)

where

is the face vector area.

Important

User-defined scalars in solid zones do not take into account the convective term with

moving reference frames.

For multiphase flows, ANSYS Fluent solves transport equations for two types of scalars: per phase

and mixture. For an arbitrary  scalar in phase-l, denoted by

, ANSYS Fluent solves the transport

equation inside the volume occupied by phase-l

(.)

Modeling Basic Fluid Flow

where

,

, and

are the volume fraction, physical density, and velocity of phase-l, respectively.

and

are the diffusion coefficient and source term, respectively, which you will need to specify. In

this case, scalar

is associated only with one phase (phase-l) and is considered an individual field

variable of phase-l.

The mass flux for phase-l is defined as

(.)

If the transport variable described by scalar

represents the physical field that is shared between

phases, or is considered the same for each phase, then you should consider this scalar as being asso-

ciated with a mixture of phases,

. In this case, the generic transport equation for the scalar is

(.)

where mixture density

, mixture velocity

, and mixture diffusivity for the scalar

are calculated

according to

(.)

(.)

(.)

(.)

(.)

To calculate mixture diffusivity, you must specify individual diffusivities for each material associated

with individual phases.

(.)

(.)

(.)

(.)

(.)

Note that if the user-defined mass flux option is activated, then mass fluxes shown in Equa-

tion . (p. ) and Equation . (p. ) must be replaced in the corresponding scalar transport

equations. For more information about the theoretical background of user-defined scalar transport

equations, see User-Defined Scalar (UDS) Transport Equations in the Theory Guide.

ANSYS Fluent allows you to define up to

user-defined scalar (UDS) transport equations in your

model. The general scalar transport equation, Equation . in the Theory Guide, is shown below with

the four terms (transient, flux, diffusivity, source) that you can customize. (Equation . (p. )). You

will define a UDS transport equation by setting the parameters for these four terms.

(.)

User-Defined Scalar (UDS) Transport Equations

In addition, you can set boundary conditions for the variables within cells of a fluid or solid zone for

a particular scalar equation. This is done by fixing the value of

in Equation . (p. ). When

is fixed in a given cell, the UDS scalar transport is not solved and the cell is not included when the

residual sum is computed. Additionally, you can also specify custom boundary conditions in the mixture

on all wall, inflow, and outflow boundaries on a per-scalar basis.

The procedures for setting up a user-defined scalar (UDS) equation for single-phase and multiphase

flows are outlined below. Note that a significant difference between a UDS for a single-phase versus

a multiphase application is that you must associate each UDS with its corresponding phase domain

or mixture domain, depending on your application. If you supply UDFs for transient terms, convective

fluxes, and sources, you must be aware that they are directly called from the phase or mixture domains,

according to the scalar association settings.

When setting up a UDS, ensure that the scalar transport problem is well defined with proper Dirich-

let/Neumann boundary conditions. Depending on the nature of the problem, the UDS equation may

need to converge further than the default convergence criterion of .. Set the convergence criterion

according to your needs.

In some instances, the residuals may not reflect the quality of the solution. In these cases you should

create monitors on the UDS and use these monitors to judge solution convergence. There are several

controls that you can adjust to improve convergence, however some of these adjustments can increase

the computation time. The following controls can help with convergence:

Using a fixed cycle, such as F-Cycle in place of Flexible cycle in the Advanced Solution Controls dialog

box.

Using an additional stabilizer such as the Biconjugate gradient stabilization method.

Using an ILU smoother.

Increasing the pre- and post-sweeps available in the Advanced Solution Controls dialog box.

Adjusting the under relaxation factors.

See the Fluent Customization Manual for information on using UDFs to define scalar quantities.

. Specify the number of UDS equations you require in the User-Defined Scalars Dialog Box (p. ) (Fig-

ure . :The User-Defined Scalars Dialog Box (p. )).

Parameters & Customization → User Defined Scalars

New...

Important

The maximum number of user-defined scalar transport equations you can define is .

ANSYS Fluent assigns numbers to the equations starting with .

Important

Note that ANSYS Fluent assigns a default name for each scalar equation (User

Scalar , User Scalar , and so on). These labels will appear in graphics dialog

boxes in ANSYS Fluent. You can change them by means of a UDF. See the Fluent Cus-

Figure . : The User-Defined Scalars Dialog Box

. Enable Inlet Diffusion if you want to include the diffusion term in the UDS transport equation for all

inflow and outflow boundaries.

. Set the first user-defined scalar equation parameters by making sure that the UDS Index is set to .

a.

Specify the Solution Zones you want the scalar equation to be solved in as all fluid zones, all solid

zones, all zones (fluid and solid) or selected zones. If you choose selected zones, click the Edit

button to view the list of zones you can select.

b. Specify the Flux Function to be none, mass flow rate, or a user-defined function (UDF).The Flux

Function determines how the convective flux is computed, which determines the equation that

ANSYS Fluent solves for the user-defined scalar. Selecting none, mass flow rate, or a user-defined

function results in ANSYS Fluent solving Equation ., Equation ., or Equation ., respectively

(in the Theory Guide). See the Fluent Customization Manual for details on flux UDFs.

c.

c.

Specify the Unsteady Function to be none, default, or a user-defined function (UDF). Select none

for a steady state solution and default if you want the transient term in Equation . in the Theory

Guide). See the separate Fluent Customization Manual for details on unsteady UDFs.

d. Repeat this process for each scalar equation by incrementing the UDS Index.

e. Click OK when all user scalar equations have been defined.

. To specify source term(s) for each of the

UDS equations, enable the Source Terms option in the Fluid

or Solid dialog box (Figure . :The Fluid Dialog Box with Inputs for Source Terms for a User-Defined

Scalar (p. )) and click the Source Terms tab.The source parameters will be displayed.

Setup →

Figure . : The Fluid Dialog Box with Inputs for Source Terms for a User-Defined Scalar

a.

Specify the number of sources you require for each scalar equation by clicking on the Edit... button

next to the scalar name (for example, User Scalar ).This will open the User Scalar  sources dialog

box (Figure . :The User Scalar Sources Dialog Box (p. )).

Figure . : The User Scalar Sources Dialog Box

b. Specify the Number of User Scalar Sources for the scalar equation by incrementing the counter.

Based on the value you have chosen, the sources will be added to the list in the dialog box. Specify

each source to be none, constant, or a user-defined function (UDF). For details on defining a UDF

scalar source, see the Fluent Customization Manual. Click OK when you have specified all scalar

sources.

. To specify diffusivity for each of the

sources.

UDS equations, display the Materials Task Page (p. ) (Fig-

ure . :The Materials Dialog Box with Input for Diffusivity for UDS Equations (p. )) and select either

defined-per-uds (the default) or user-defined in the drop-down list for UDS Diffusivity.

Setup →

Materials → Create/Edit

Figure . : The Materials Dialog Box with Input for Diffusivity for UDS Equations

See User-Defined Scalar (UDS) Diffusivity (p. ) for details on the different options available to

you for defining diffusion coefficients.

. To specify boundary conditions for the user-defined scalars on wall, inflow, and outflow boundaries, you

can define a specific value or a specific flux for each scalar. A coupled boundary condition can be specified

on two-sided walls for scalars that are to be solved in regions on both sides of the wall (that is, scalars

solved in both fluid and solid zones).

Setup →

a.

In the UDS tab under User Defined Scalar Boundary Condition, select either Specified Flux or

Specified Value in the drop-down list next to each scalar (for example, User Scalar ) for a boundary

wall. For interior walls, select Coupled Boundary if the scalars are to be solved on both sides of a

two-sided wall. Note that the Coupled Boundary option will only show up in the drop-down list if

the scalar is defined in the fluid and solid zones in the User-Defined Scalars Dialog Box (p. ).

b. Under User Defined Scalar Boundary Value, enter a constant value or select a user-defined function

from the drop-down list for each scalar. If you select Specified Flux, your input will be the value of

the flux at the boundary (that is, the negative of the term in parenthesis on the left-hand side of in

the Theory Guide) dot [as in the dot product of]  [as in the vector, n], where  is the normal into the

domain). If you select Specified Value, your input will be the value of the scalar itself at the boundary.

See the Fluent Customization Manual for information on using UDFs for UDS boundary conditions.

. Set the solution parameters in the Solution Controls task page, specify an initial value for each UDS (as

you do for all other scalar transport equations), and calculate a solution.

. Examine the results using the usual postprocessing tools. In each postprocessing dialog box, the list of

field variables will include the User Defined Scalars... category, which contains the value of each UDS

and its diffusion coefficient (

in Equation ., Equation ., Equation ., or Equation . (in the

Theory Guide):

User Scalar-n

Diffusion Coef. of Scalar-n

. Specify the number of scalars in the User-Defined Scalars Dialog Box (p. ) (Figure . :The User-Defined

Scalars Dialog Box for a Multiphase Flow (p. )).

New...

Figure . : The User-Defined Scalars Dialog Box for a Multiphase Flow

Important

ANSYS Fluent assigns numbers to the equations starting with . The default association

type is set to mixture for all scalars.

Important

Important

. Keep the default Inlet Diffusion enabled if you want to include the diffusion term in the UDS transport

equation for all inflow and outflow boundaries.

a.

Select the Phase you want the scalar equation solved in as a primary phase, secondary phase, or the

mixture.

b. Specify the Solution Zones you want the scalar equation to be solved in as all fluid zones, all solid

c.

Specify the Flux Function to Unsteady Function the same way as you would for a single phase flow

(see above).

. Specify source term(s) for each of the

UDS equations in the Fluid or Solid dialog box as described for

a single phase flow (see above).

. Specify boundary conditions for the user-defined scalars in the mixture on all wall, inflow, and outflow

boundary as described for a single phase flow (see above).

. Set the solution parameters, specify an initial value for each UDS (as you do for all other scalar transport

equations), and calculate a solution.

Periodic flow occurs when the physical geometry of interest and the expected pattern of the flow/thermal

solution have a periodically repeating nature. Two types of periodic flow can be modeled in ANSYS

Fluent. In the first type, no pressure drop occurs across the periodic planes. In the second type, a pressure

drop occurs across translationally periodic boundaries, resulting in “fully-developed” or “streamwise-

periodic” flow.

This section discusses streamwise-periodic flow. A description of no-pressure-drop periodic flow is

provided in Periodic Boundary Conditions (p. ), and a description of streamwise-periodic heat transfer

is provided in Modeling Periodic Heat Transfer (p. ).

Information about streamwise-periodic flow is presented in the following sections:

... Overview and Limitations

... User Inputs for the Pressure-Based Solver

... User Inputs for the Density-Based Solvers

... Monitoring the Value of the Pressure Gradient

... Postprocessing for Streamwise-Periodic Flows

For more information about the theoretical background of periodic flows, see Periodic Flows in the

More information about periodic flows is presented in the following sections:

.... Limitations for Modeling Streamwise-Periodic Flow

ANSYS Fluent provides the ability to calculate streamwise-periodic—or “fully-developed”—fluid flow.

These flows are encountered in a variety of applications, including flows in compact heat exchanger

channels and flows across tube banks. In such flow configurations, the geometry varies in a repeating

manner along the direction of the flow, leading to a periodic fully-developed flow regime in which

the flow pattern repeats in successive cycles. Other examples of streamwise-periodic flows include

fully-developed flow in pipes and ducts. These periodic conditions are achieved after a sufficient en-

trance length, which depends on the flow Reynolds number and geometric configuration.

Streamwise-periodic flow conditions exist when the flow pattern repeats over some length , with a

constant pressure drop across each repeating module along the streamwise direction. Figure . : Ex-

ample of Periodic Flow in a 2D Heat Exchanger Geometry (p. ) depicts one example of a periodically

repeating flow of this type that has been modeled by including a single representative module.

Figure . : Example of Periodic Flow in a 2D Heat Exchanger Geometry

The following limitations apply to modeling streamwise-periodic flow:

The flow must be incompressible.

When performing unsteady-state simulations with translational periodic boundary conditions, the specified

pressure gradient is recommended.

If one of the density-based solvers is used, you can specify only the pressure jump; for the pressure-based

solver, you can specify either the pressure jump or the mass flow rate.

Periodic Flows

No net mass addition through inlets/exits or extra source terms is allowed.

Species can be modeled only if inlets/exits (without net mass addition) are included in the problem. Re-

acting flows are not permitted.

When you specify a periodic mass-flow rate, Fluent will assume that the entire flow rate passes

through one periodic continuous face zone only.

Steady particle tracks can be modeled only if the particles have a possibility to leave the domain without

generating incomplete trajectories.

While multiphase flow can be modeled with translational periodic boundary conditions, you cannot

use the mass flow rate specification method. However, you can specify a constant pressure gradient.

For periodic simulations that include heat transfer, see also the limitations described in Constraints

for Periodic Heat Transfer Predictions (p. ).

If you are using the pressure-based solver, in order to calculate a spatially periodic flow field with a

specified mass flow rate or pressure derivative, you must first create a mesh with translationally peri-

odic boundaries that are parallel to each other and equal in size. You can specify translational periodicity

in the Periodic Conditions Dialog Box (p. ), as described in Periodic Boundary Conditions (p. ). (If

you need to create periodic boundaries, see Creating Periodic Zones and Interfaces (p. )).

In the Periodic Conditions Dialog Box (p. ) that is opened from the Boundary Conditions Task

Page (p. ), you will complete the following inputs after the mesh has been read into ANSYS Fluent

(Figure . : The Periodic Conditions Dialog Box (p. )):

Setup →

Figure . : The Periodic Conditions Dialog Box

Setup →

. Select either the specified mass flow rate (Specify Mass Flow) option or the specified pressure gradient

(Specify Pressure Gradient) option. For most problems, the mass flow rate across the periodic boundary

will be a known quantity; for others, the mass flow rate will be unknown, but the pressure gradient (  in

Equation ., in the Theory Guide) will be a known quantity.

. Specify the mass flow rate and/or the pressure gradient (  in Equation ., in the Theory Guide):

If you selected the Specify Mass Flow option, enter the desired value for the Mass Flow Rate.You can

also specify an initial guess for the Pressure Gradient, but this is not required.

Important

For axisymmetric problems, the mass flow rate is per

radians.

If you selected the Specify Pressure Gradient option, enter the desired value for Pressure Gradient.

. Define the flow direction by setting the X,Y,Z (or X,Y in 2D) point under Flow Direction.The flow will

move in the direction of the vector pointing from the origin to the specified point.The direction vector

must be parallel to the periodic translation direction or its opposite.

. If you chose in step  to specify the mass flow rate, set the parameters used for the calculation of .These

parameters are described in detail below.

After completing these inputs, you can solve the periodic velocity field to convergence.

.... Setting Parameters for the Calculation of β

If you choose to specify the mass flow rate, ANSYS Fluent must calculate the appropriate value of the

pressure gradient . You can control this calculation by specifying the Relaxation Factor and the

Number of Iterations, and by supplying an initial guess for . All of these inputs are entered in the

Periodic Conditions Dialog Box (p. ).

The Number of Iterations sets the number of sub-iterations performed on the correction of  in the

pressure correction equation. Because the value of  is not known a priori, it must be iterated on

until the Mass Flow Rate that you have defined is achieved in the computational model. This correction

of  occurs in the pressure correction step of the SIMPLE, SIMPLEC, or PISO algorithm. A correction

to the current value of  is calculated based on the difference between the desired mass flow rate

and the actual one. The sub-iterations referred to here are performed within the pressure correction

step to improve the correction for  before the pressure correction equation is solved for the resulting

pressure (and velocity) correction values. The default value of  sub-iterations should suffice in most

problems, but can be increased to help speed convergence. The Relaxation Factor is an under-relax-

ation factor that controls convergence of this iteration process.

You can also speed up convergence of the periodic calculation by supplying an initial guess for  in

the Pressure Gradient field. Note that the current value of  will be displayed in this field if you

have performed any calculations. To update the Pressure Gradient field with the current value at

any time, click the Update button.

If you are using one of the density-based solvers, in order to calculate a spatially periodic flow field

with a specified pressure jump, you must first create a mesh with translationally periodic boundaries

that are parallel to each other and equal in size. (If you need to create periodic boundaries, see Creating

Periodic Zones and Interfaces (p. ).)

Then, follow the steps below:

. In the Periodic Dialog Box (p. ) (Figure . :The Periodic Dialog Box (p. )), which is opened from the

Boundary Conditions task page, indicate that the periodicity is Translational (the default).

Setup →

Periodic → Edit...

. Also in the Periodic Dialog Box (p. ), set the Periodic Pressure Jump (

in Equation . in the Theory

Guide).

If you have specified the mass flow rate, you can monitor the value of the pressure gradient  during

the calculation by creating a report plot that includes periodic pressure gradient, to ensure that you

reach a converged solution. See Monitoring Statistics (p. ) for additional information.

For streamwise-periodic flows, the velocity field should be completely periodic. If a density-based

solver is used to compute the periodic flow, the pressure field reported will be the actual pressure

(which is not periodic). If the pressure-based solver is used, the pressure field reported will be the

periodic pressure field

of Equation ., in the Theory Guide. Figure . : Periodic Pressure Field

Predicted for Flow in a 2D Heat Exchanger Geometry (p. ) displays the periodic pressure field in the

geometry of Figure . : Example of Periodic Flow in a 2D Heat Exchanger Geometry (p. ).

If you specified a mass flow rate and had ANSYS Fluent calculate the pressure gradient, you can check

the pressure gradient in the streamwise direction ( ) by looking at the current value for Pressure

Gradient in the Periodic Conditions Dialog Box (p. ).

Figure . : Periodic Pressure Field Predicted for Flow in a 2D Heat Exchanger Geometry

Many important engineering flows involve swirl or rotation and ANSYS Fluent is well-equipped to

model such flows. Swirling flows are common in combustion, with swirl introduced in burners and

combustors in order to increase residence time and stabilize the flow pattern. Rotating flows are also

encountered in turbomachinery, mixing tanks, and a variety of other applications.

Information about rotating and swirling flows is provided in the following subsections:

... Overview of Swirling and Rotating Flows

...Turbulence Modeling in Swirling Flows

... Mesh Setup for Swirling and Rotating Flows

... Modeling Axisymmetric Flows with Swirl or Rotation

For more information about the theoretical background of swirling and rotating flows, see Swirling and

Rotating Flows in the Theory Guide.

When you begin the analysis of a rotating or swirling flow, it is essential that you classify your problem

into one of the following five categories of flow:

axisymmetric flows with swirl or rotation

fully three-dimensional swirling or rotating flows

flows requiring a moving reference frame

Swirling and Rotating Flows

flows requiring multiple moving reference frames or mixing planes

flows requiring sliding meshes

Modeling and solution procedures for the first two categories are presented in this section. The remaining

three, which all involve “moving zones”, are discussed in Modeling Flows with Moving Reference

Frames (p. ).

An overview of swirling and rotating flows is presented in the following sections:

.... Axisymmetric Flows with Swirl or Rotation

....Three-Dimensional Swirling Flows

.... Flows Requiring a Moving Reference Frame

Your problem may be axisymmetric with respect to geometry and flow conditions but still include

swirl or rotation. In this case, you can model the flow in 2D (that is, solve the axisymmetric problem)

and include the prediction of the circumferential (or swirl) velocity. It is important to note that while

the assumption of axisymmetry implies that there are no circumferential gradients in the flow, there

may still be nonzero swirl velocities.

..... Momentum Conservation Equation for Swirl Velocity

The tangential momentum equation for 2D swirling flows may be written as

(.)

where  is the axial coordinate,  is the radial coordinate,

is the axial velocity,

is the radial velocity,

and

is the swirl velocity.

When there are geometric changes and/or flow gradients in the circumferential direction, your swirling

and

flow prediction requires a three-dimensional model. If you are planning a 3D ANSYS Fluent model

that includes swirl or rotation, you should be aware of the setup constraints listed in Coordinate

System Restrictions (p. ). In addition, you might consider simplifications to the problem that might

reduce it to an equivalent axisymmetric problem, especially for your initial modeling effort. Because

of the complexity of swirling flows, an initial 2D study, in which you can quickly determine the effects

of various modeling and design choices, can be very beneficial.

Important

For 3D problems involving swirl or rotation, there are no special inputs required during

the problem setup and no special solution procedures. Note, however, that you may want

to use the cylindrical coordinate system for defining velocity-inlet boundary condition inputs,

as described in Defining the Velocity (p. ). Also, you may find the gradual increase of

the rotational speed (set as a wall or inlet boundary condition) helpful during the solution

process. This is described for axisymmetric swirling flows in Improving Solution Stability

by Gradually Increasing the Rotational or Swirl Speed (p. ).

If your flow involves a rotating boundary that moves through the fluid (for example, an impeller blade

or a grooved or notched surface), you must use a moving reference frame to model the problem.

Such applications are described in detail in Introduction (p. ). If you have more than one rotating

boundary (for example, several impellers in a row), you can use multiple reference frames (described

in The Multiple Reference Frame Model (p. )) or mixing planes (described in The Mixing Plane

Model (p. )).

If you are modeling turbulent flow with a significant amount of swirl (for example, cyclone flows,

swirling jets), you should consider using one of ANSYS Fluent’s advanced turbulence models: the RNG

model, realizable -  model, or Reynolds stress model. The appropriate choice depends on the

strength of the swirl, which can be gauged by the swirl number. The swirl number is defined as the

ratio of the axial flux of angular momentum to the axial flux of axial momentum:

(.)

where  is the hydraulic radius.

For flows with weak to moderate swirl (

), both the RNG -  model and the realizable -

model yield appreciable improvements over the standard -  model. See RNG k-ε Model and Realizable

k-ε Model Swirl Modification (p. ) for details about these models.

For highly swirling flows (

), the Reynolds stress model (RSM) is strongly recommended. The effects

of strong turbulence anisotropy can be modeled rigorously only by the second-moment closure adopted

in the RSM. See Reynolds Stress Model (RSM) Steps in Using a Turbulence Model (p. ) for details

about this model.

For swirling flows encountered in devices such as cyclone separators and swirl combustors, near-wall

turbulence modeling is quite often a secondary issue at most. The fidelity of the predictions in these

cases is mainly determined by the accuracy of the turbulence model in the core region. However, in

cases where walls actively participate in the generation of swirl (that is, where the secondary flows

and vortical flows are generated by pressure gradients), non-equilibrium wall functions can often improve

the predictions since they use a law of the wall for mean velocity sensitized to pressure gradients. See

Near-Wall Treatments for Wall-Bounded Turbulent Flows in the Theory Guide for additional details

about near-wall treatments for turbulence.

.... Coordinate System Restrictions

Recall that for an axisymmetric problem, the axis of rotation must be the  axis and the mesh must

lie on or above the

line.

.... Mesh Sensitivity in Swirling and Rotating Flows

In addition to the setup constraint described above, you should be aware of the need for sufficient

resolution in your mesh when solving flows that include swirl or rotation. Typically, rotating boundary

layers may be very thin, and your ANSYS Fluent model will require a very fine mesh near a rotating

wall. In addition, swirling flows will often involve steep gradients in the circumferential velocity (for

example, near the centerline of a free-vortex type flow), and therefore require a fine mesh for accurate

resolution.

As discussed in Overview of Swirling and Rotating Flows (p. ), you can solve a 2D axisymmetric

problem that includes the prediction of the circumferential or swirl velocity. The assumption of

axisymmetry implies that there are no circumferential gradients in the flow, but that there may be

nonzero circumferential velocities. Examples of axisymmetric flows involving swirl or rotation are de-

picted in Figure . : Rotating Flow in a Cavity (p. ) and Figure . : Swirling Flow in a Gas Burn-

er (p. ).

Figure . : Rotating Flow in a Cavity

Figure . : Swirling Flow in a Gas Burner

.... Problem Setup for Axisymmetric Swirling Flows

For axisymmetric problems, you must perform the following steps during the problem setup procedure.

(Only those steps relevant specifically to the setup of axisymmetric swirl/rotation are listed here. You

must set up the rest of the problem as usual.)

. Enable the solution of the momentum equation in the circumferential direction by turning on the

Axisymmetric Swirl option for Space in the General task page.

Setup →

General →

Axisymmetric Swirl

. Define the rotational or swirling component of velocity,

, at inlets or walls.

Setup →

Important

Remember to use the axis boundary type for the axis of rotation.

The procedures for input of rotational velocities at inlets and at walls are described in detail in Defining

the Velocity (p. ) and  Velocity Conditions for Moving Walls (p. ).

.... Solution Strategies for Axisymmetric Swirling Flows

The difficulties associated with solving swirling and rotating flows are a result of the high degree of

coupling between the momentum equations, which is introduced when the influence of the rotational

terms is large. A high level of rotation introduces a large radial pressure gradient that drives the flow

in the axial and radial directions. This, in turn, determines the distribution of the swirl or rotation in

the field. This coupling may lead to instabilities in the solution process, and you may require special

solution techniques in order to obtain a converged solution. Solution techniques that may be bene-

ficial in swirling or rotating flow calculations include the following:

(Pressure-based segregated solver only) Use the PRESTO! scheme (enabled in the Pressure list for Spatial

Discretization in the Solution Methods Task Page (p. )), which is well-suited for the steep pressure

gradients involved in swirling flows.

Ensure that the mesh is sufficiently refined to resolve large gradients in pressure and swirl velocity.

(Pressure-based solver only) Change the under-relaxation parameters on the velocities, perhaps to .–.

for the radial and axial velocities and .–. for swirl.

(Pressure-based solver only) Use a sequential or step-by-step solution procedure, in which some equations

are temporarily left inactive (see below).

If necessary, start the calculations using a low rotational speed or inlet swirl velocity, increasing the rotation

or swirl gradually in order to reach the final desired operating condition (see below).

See Using the Solver (p. ) for details on the procedures used to make these changes to the solution

parameters. More details on the step-by-step procedure and on the gradual increase of the rotational

speed are provided below.

..... Step-By-Step Solution Procedures for Axisymmetric Swirling Flows

Often, flows with a high degree of swirl or rotation will be easier to solve if you use the following

step-by-step solution procedure, in which only selected equations are left active in each step. This

approach allows you to establish the field of angular momentum, then leave it fixed while you update

the velocity field, and then finally to couple the two fields by solving all equations simultaneously.

Important

Since the density-based solvers solve all the flow equations simultaneously, the following

procedure applies only to the pressure-based solver.

In this procedure, you will use the Equations... button in the Solution Controls Task Page (p. ) to

turn individual transport equations on and off between calculations.

. If your problem involves inflow/outflow, begin by solving the flow without rotation or swirl effects.That

is, enable the Axisymmetric option instead of the Axisymmetric Swirl option in the General Task

Page (p. ), and do not set any rotating boundary conditions.The resulting flow-field data can be used

as a starting guess for the full problem.

. Enable the Axisymmetric Swirl option and set all rotating/swirling boundary conditions.

. Begin the prediction of the rotating/swirling flow by solving only the momentum equation describing

the circumferential velocity.This is the Swirl Velocity listed in the Equations list in the Equations Dialog

Box (p. ). Let the rotation “diffuse” throughout the flow field, based on your boundary condition inputs.

In a turbulent flow simulation, you may also want to leave the turbulence equations active during this

step.This step will establish the field of rotation throughout the domain.

. Turn off the momentum equations describing the circumferential motion (Swirl Velocity). Leaving the

velocity in the circumferential direction fixed, solve the momentum and continuity (pressure) equations

(Flow in the Equations list in the Equations Dialog Box (p. )) in the other coordinate directions.This

step will establish the axial and radial flows that are a result of the rotation in the field. Again, if your

problem involves turbulent flow, you should leave the turbulence equations active during this calculation.

. Turn on all of the equations simultaneously to obtain a fully coupled solution. Note the under-relaxation

controls suggested above.

In addition to the steps above, you may want to simplify your calculation by solving isothermal flow

before adding heat transfer or by solving laminar flow before adding a turbulence model. These two

methods can be used for any of the solvers (that is, pressure-based or density-based).

..... Improving Solution Stability by Gradually Increasing the Rotational or Swirl

Speed

Because the rotation or swirl defined by the boundary conditions can lead to large complex forces

in the flow, your ANSYS Fluent calculations will be less stable as the speed of rotation or degree of

swirl increases. Hence, one of the most effective controls you can apply to the solution is to solve

your rotating flow problem starting with a low rotational speed or swirl velocity and then slowly

increase the magnitude up to the desired level. The procedure for accomplishing this is as follows:

. Set up the problem using a low rotational speed or swirl velocity in your inputs for boundary conditions.

The rotation or swirl in this first attempt might be selected as % of the actual operating conditions.

. Solve the problem at these conditions, perhaps using the step-by-step solution strategy outlined above.

. Save this initial solution data.

. Modify your inputs (boundary conditions). Increase the speed of rotation, perhaps doubling it.

. Restart the calculation using the solution data saved in step  as the initial solution for the new calcula-

tion. Save the new data.

. Continue to increment the speed of rotation, following steps  and , until you reach the desired oper-

ating condition.

...... Postprocessing for Axisymmetric Swirling Flows

Reporting of results for axisymmetric swirling flows is the same as for other flows. The following

additional variables are available for postprocessing when axisymmetric swirl is active:

Swirl Velocity (in the Velocity... category)

Swirl-Wall Shear Stress (in the Wall Fluxes... category)

Compressibility effects are encountered in gas flows at high velocity and/or in which there are large

pressure variations. When the flow velocity approaches or exceeds the speed of sound of the gas or

when the pressure change in the system (

) is large, the variation of the gas density with pressure

has a significant impact on the flow velocity, pressure, and temperature. Compressible flows create a

unique set of flow physics for which you must be aware of the special input requirements and solution

techniques described in this section. Figure . : Flow in a Converging-Diverging Nozzle (p. ) shows

compressible flows computed using ANSYS Fluent.

Compressible Flows

Figure . : Flow in a Converging-Diverging Nozzle

Information about compressible flows is provided in the following subsections:

...When to Use the Compressible Flow Model

... Physics of Compressible Flows

... Modeling Inputs for Compressible Flows

... Floating Operating Pressure

... Solution Strategies for Compressible Flows

... Reporting of Results for Compressible Flows

For more information about the theoretical background of compressible flows, see Compressible Flows

in the Theory Guide.

Compressible flows can be characterized by the value of the Mach number:

(.)

Here,  is the speed of sound in the gas:

(.)

and  is the ratio of specific heats

.

When the Mach number is less than ., the flow is termed subsonic. At Mach numbers much less than

. (

or so), compressibility effects are negligible and the variation of the gas density with pressure

can safely be ignored in your flow modeling. As the Mach number approaches . (which is referred

to as the transonic flow regime), compressibility effects become important. When the Mach number

exceeds ., the flow is termed supersonic, and may contain shocks and expansion fans which can

impact the flow pattern significantly. ANSYS Fluent provides a wide range of compressible flow mod-

eling capabilities for subsonic, transonic, and supersonic flows.

Compressible flows are typically characterized by the total pressure

and total temperature

of the

flow. For an ideal gas, these quantities can be related to the static pressure and temperature by the

(.)

For constant

, Equation . (p. ) reduces to

(.)

These relationships describe the variation of the static pressure and temperature in the flow as the

velocity (Mach number) changes under isentropic conditions. For example, given a pressure ratio from

inlet to exit (total to static), Equation . (p. ) can be used to estimate the exit Mach number that

would exist in a one-dimensional isentropic flow. For air, Equation . (p. )

, of .. This

choked flow condition will be established at the point of minimum flow area (for example, in the throat

of a nozzle). In the subsequent area expansion the flow may either accelerate to a supersonic flow in

which the pressure will continue to drop, or return to subsonic flow conditions, decelerating with a

pressure rise. If a supersonic flow is exposed to an imposed pressure increase, a shock will occur, with

a sudden pressure rise and deceleration accomplished across the shock.

.... Basic Equations for Compressible Flows

Compressible flows are described by the standard continuity and momentum equations solved by

ANSYS Fluent, and you do not need to enable any special physical models (other than the compressible

treatment of density as detailed below). The energy equation solved by ANSYS Fluent correctly incor-

porates the coupling between the flow velocity and the static temperature, and should be activated

whenever you are solving a compressible flow. In addition, if you are using the pressure-based solver,

you should enable the viscous dissipation terms in Equation . in the Theory Guide, which become

important in high-Mach-number flows.

....The Compressible Form of the Gas Law

For compressible flows, the ideal gas law is written in the following form:

(.)

where

is the operating pressure defined in the Operating Conditions Dialog Box (p. ),

is the

local static pressure relative to the operating pressure,

is the universal gas constant, and

is the

molecular weight. The temperature,

, will be computed from the energy equation.

Some compressible flow problems involve fluids that do not behave as ideal gases. For example, flow

under very high-pressure conditions cannot typically be modeled accurately using the ideal-gas as-

sumption. Therefore, the real gas model described in Real Gas Models (p. ) should be used instead.

To set up a compressible flow in ANSYS Fluent, you must follow the steps listed below. (Only those

steps relevant specifically to the setup of compressible flows are listed here. You must set up the rest

of the problem as usual.)

. Set the Operating Pressure in the Operating Conditions Dialog Box (p. ).

Setup →

(You can think of

as the absolute static pressure at a point in the flow where you will define

the gauge pressure  to be zero. See Operating Pressure (p. ) for guidelines on setting the oper-

ating pressure. For time-dependent compressible flows, you may want to specify a floating operating

pressure instead of a constant operating pressure. See Floating Operating Pressure (p. ) for details.)

. Enable the solution of the energy equation.

Setup → Models → Energy

On

. (Pressure-based solver only) If you are modeling turbulent flow, enable the optional viscous dissipation

terms in the energy equation by turning on Viscous Heating in the Viscous Model Dialog Box (p. ).

Note that these terms can be important in high-speed flows.

Setup →

Models →

Viscous → Edit...

This step is not necessary if you are using one of the density-based solvers, because the density-

based solvers always include the viscous dissipation terms in the energy equation.

. Set the following items in the Create/Edit Materials Dialog Box (p. ):

Setup →

a.

Select ideal-gas in the drop-down list next to Density.

b. Define all relevant properties (specific heat, molecular weight, thermal conductivity, and so on).

. Set cell zone conditions and boundary conditions (using the Boundary Conditions Task Page (p. ) and

Cell Zone Conditions Task Page (p. )), being sure to choose a well-posed cell zone or boundary condition

combination that is appropriate for the flow regime. See below for details. Recall that all inputs for pressure

(either total pressure or static pressure) must be relative to the operating pressure, and the temperature

inputs at inlets should be total (stagnation) temperatures, not static temperatures.

Setup →

Setup →

Setup →

Setup →

These inputs should ensure a well-posed compressible flow problem. You will also want to consider

special solution parameter settings, as noted in Solution Strategies for Compressible Flows (p. ),

before beginning the flow calculation.

.... Boundary Conditions for Compressible Flows

Well-posed inlet and exit boundary conditions for compressible flow are listed below:

For flow inlets:

– Pressure inlet: Inlet total temperature and total pressure and, for supersonic inlets, static pressure

– Mass-flow inlet: Inlet mass flow and total temperature

For flow exits:

– Pressure outlet: Exit static pressure (ignored if flow is supersonic at the exit. All the information travels

downstream in a supersonic region, hence the pressure at the outlet can be computed by directly ex-

trapolating from the adjacent cell center  [] (p. ).Therefore, it is not meaningful to use the exit

static pressure prescribed in the boundary conditions task page, and the exit static pressure is ignored).

– Mass-flow outlet: Outlet mass flow

It is important to note that your boundary condition inputs for pressure (either total pressure or

static pressure) must be in terms of gauge pressure — that is, pressure relative to the operating

pressure defined in the Operating Conditions Dialog Box (p. ), as described above.

All temperature inputs at inlets should be total (stagnation) temperatures, not static temperatures.

ANSYS Fluent provides a “floating operating pressure” option to handle time-dependent compressible

flows with a gradual increase in the absolute pressure in the domain. This option is desirable for slow

subsonic flows with static pressure build-up, since it efficiently accounts for the slow changing of ab-

solute pressure without using acoustic waves as the transport mechanism for the pressure build-up.

Examples of typical applications include the following:

combustion or heating of a gas in a closed domain

pumping of a gas into a closed domain

The floating operating pressure option should not be used for transonic or incompressible flows. In

addition, it cannot be used if your model includes any pressure inlet, pressure outlet, exhaust fan,

inlet vent, intake fan, outlet vent, or pressure far field boundaries.

The floating operating pressure option allows ANSYS Fluent to calculate the pressure rise (or drop)

from the integral mass balance, separately from the solution of the pressure correction equation.

When this option is activated, the absolute pressure at each iteration can be expressed as

(.)

where  is the pressure relative to the reference location, which in this case is in the cell with the

minimum pressure value. Therefore the reference location itself is floating.

is referred to as the floating operating pressure, and is defined as

(.)

where

is the initial operating pressure and

is the pressure rise.

Including the pressure rise

in the floating operating pressure

, rather than in the pressure

, helps to prevent roundoff error. If the pressure rise were included in , the calculation of the

pressure gradient for the momentum equation would give an inexact balance due to precision limits

for -bit real numbers.

.... Enabling Floating Operating Pressure

When time dependence is active, you can turn on the Floating Operating Pressure option in the

Operating Conditions Dialog Box (p. ).

Setup →

(Note that the inputs for Reference Pressure Location will disappear when you enable Floating

Operating Pressure, since these inputs are no longer relevant.)

Important

The floating operating pressure option should not be used for transonic flows or for incom-

pressible flows. It is meaningful only for slow subsonic flows of ideal gases, when the

characteristic time scale is much larger than the sonic time scale.

.... Setting the Initial Value for the Floating Operating Pressure

When the floating operating pressure option is enabled, you must specify a value for the Initial Op-

erating Pressure in the Solution Initialization Task Page (p. ).

Solution →

Initialization

This initial value is stored in the case file with all your other initial values.

.... Storage and Reporting of the Floating Operating Pressure

The current value of the floating operating pressure is stored in the data file. If you visit the Operating

Conditions Dialog Box (p. ) after a number of time steps have been performed, the current value

of the Operating Pressure will be displayed.

Note that the floating operating pressure will automatically be reset to the initial operating pressure

if you reset the data (that is, start over at the first iteration of the first time step).

.... Monitoring Absolute Pressure

You can monitor the absolute pressure during the calculation using the Surface Report Definition

Dialog Box (p. ). You can also generate graphical plots or alphanumeric reports of absolute pressure

when your solution is complete. The Absolute Pressure variable is contained in the Pressure... cat-

egory of the variable selection drop-down list that appears in postprocessing dialog boxes. See Field

Function Definitions (p. ) for its definition.

The difficulties associated with solving compressible flows are a result of the high degree of coupling

between the flow velocity, density, pressure, and energy. This coupling may lead to instabilities in the

solution process and, therefore, may require special solution techniques in order to obtain a converged

solution. In addition, the presence of shocks (discontinuities) in the flow introduces an additional sta-

bility problem during the calculation. Solution techniques that may be beneficial in compressible flow

calculations include the following:

(Pressure-based solver only) Initialize the flow to be near stagnation (that is velocity small but not zero,

pressure to inlet total pressure, temperature to inlet total temperature).Turn off the energy equation for

the first  iterations. Leave the energy under-relaxation at . Set the pressure under-relaxation to ., and

the momentum under-relaxation to .. After the solution stabilizes and the energy equation has been

turned on, increase the pressure under-relaxation to ..

Set reasonable limits for the temperature and pressure (in the Solution Limits Dialog Box (p. )) to avoid

solution divergence, especially at the start of the calculation. If ANSYS Fluent prints messages about tem-

perature or pressure being limited as the solution nears convergence, the high or low computed values

may be physical, and you must change the limits to allow these values.

If required, begin the calculations using a reduced pressure ratio at the boundaries, increasing the pressure

ratio gradually in order to reach the final desired operating condition. If the Mach number is low, you can

also consider starting the compressible flow calculation from an incompressible flow solution (although

the incompressible flow solution can in some cases be a rather poor initial guess for the compressible cal-

culation).

In some cases, computing an inviscid solution as a starting point may be helpful.

You can display the results of your compressible flow calculations in the same manner that you would

use for an incompressible flow. The variables listed below are of particular interest when you model

compressible flow:

These variables are contained in the variable selection drop-down list that appears in postprocessing

dialog boxes. Total Temperature is in the Temperature... category, Total Pressure is in the Pressure...

category, and Mach Number is in the Velocity... category. See Field Function Definitions (p. ) for

their definitions.

Inviscid flow analysis neglect the effect of viscosity on the flow and are appropriate for high-Reynolds-

number applications where inertial forces tend to dominate viscous forces. One example for which an

inviscid flow calculation is appropriate is an aerodynamic analysis of some high-speed projectile. In a

case like this, the pressure forces on the body will dominate the viscous forces. Hence, an inviscid ana-

lysis will give you a quick estimate of the primary forces acting on the body. After the body shape has

been modified to maximize the lift forces and minimize the drag forces, you can perform a viscous

analysis to include the effects of the fluid viscosity and turbulent viscosity on the lift and drag forces.

Another area where inviscid flow analysis are routinely used is to provide a good initial solution for

problems involving complicated flow physics and/or complicated flow geometry. In a case like this, the

viscous forces are important, but in the early stages of the calculation the viscous terms in the momentum

equations will be ignored. Once the calculation has been started and the residuals are decreasing, you

can turn on the viscous terms (by enabling laminar or turbulent flow) and continue the solution to

convergence. For some very complicated flows, this is the only way to get the calculation started.

Information about inviscid flows is provided in the following subsections:

... Setting Up an Inviscid Flow Model

... Solution Strategies for Inviscid Flows

... Postprocessing for Inviscid Flows

For more information about the theoretical background of inviscid flows, see Inviscid Flows in the

For inviscid flow problems, you must perform the following steps during the problem setup procedure.

(Only those steps relevant specifically to the setup of inviscid flow are listed here. You must set up the

rest of the problem as usual.)

. Enable the calculation of inviscid flow by selecting Inviscid in the Viscous Model Dialog Box (p. ).

→ Model → Inviscid

. Set boundary conditions and flow properties.

Setup →

Note

Walls are assumed to be slip surfaces (the velocity is not equal to zero, unlike viscous

flows) and therefore have a tangential velocity computed based on the solution of the

governing equations.

Setup →

Materials

. Solve the problem and examine the results.

Since inviscid flow problems will usually involve high-speed flow, you may have to reduce the under-

relaxation factors for momentum (if you are using the pressure-based solver) or reduce the Courant

number (if you are using the density-based solver), in order to get the solution started. Once the flow

is started and the residuals are monotonically decreasing, you can start increasing the under-relaxation

factors or Courant number back up to the default values.

Modifications to the under-relaxation factors and the Courant number can be made in the Solution

Controls Task Page (p. ).

Solution →

Controls

Solution →

Controls

The solution strategies for compressible flows apply also to inviscid flows. See Solution Strategies for

Compressible Flows (p. ) for details.

If you are interested in the lift and drag forces acting on your model, you can use the Force Reports

Dialog Box (p. ) to compute them.

Results → Reports → Forces

Edit...

See Forces on Boundaries (p. ) for details.

Inviscid Flows

Chapter : Modeling Flows with Moving Reference Frames

This chapter provides details about the moving reference frame capabilities in ANSYS Fluent.

.. Introduction

.. Flow in Single Moving Reference Frames (SRF)

.. Flow in Multiple Moving Reference Frames

ANSYS Fluent solves the equations of fluid flow and heat transfer, by default, in a stationary (or inertial)

reference frame. However, there are many problems where it is advantageous to solve the equations

in a moving (or non-inertial) reference frame. Such problems typically involve moving parts (such as

rotating blades, impellers, and similar types of moving surfaces), and it is the flow around these moving

parts that is of interest. In most cases, the moving parts render the problem unsteady when viewed

from the stationary frame. With a moving reference frame, however, the flow around the moving part

can (with certain restrictions) be modeled as a steady-state problem with respect to the moving frame.

ANSYS Fluent’s moving reference frame modeling capability allows you to model problems involving

moving parts by allowing you to enable moving reference frames in selected cell zones. When a moving

reference frame is activated, the equations of motion are modified to incorporate the additional accel-

eration terms that occur due to the transformation from the stationary to the moving reference frame.

By solving these equations in a steady-state manner, the flow around the moving parts can be modeled.

For many problems, it may be possible to refer the entire computational domain to a single moving

reference frame. This is known as the single reference frame (or SRF) approach. The use of the SRF ap-

proach is possible; provided the geometry meets certain requirements. For more complex geometries,

it may not be possible to use a single reference frame. In such cases, you must break up the problem

into multiple cell zones, with well-defined interfaces between the zones. The manner in which the in-

terfaces are treated leads to two approximate, steady-state modeling methods for this class of problem:

the multiple reference frame (or MRF) approach, and the mixing plane approach. These approaches will

be discussed in The Multiple Reference Frame Model (p. ) and The Mixing Plane Model (p. ). If

unsteady interaction between the stationary and moving parts is important, you can employ the sliding

mesh approach to capture the transient behavior of the flow. The sliding meshing model will be discussed

in Modeling Flows Using Sliding and Dynamic Meshes (p. ).

The principal reason for employing a moving reference frame is to render a problem that is unsteady

in the stationary (inertial) frame, steady with respect to the moving frame. For a steadily moving frame

(for example, the frame speed is constant), it is possible to transform the equations of fluid motion to

the moving frame such that steady-state solutions are possible. By default, ANSYS Fluent permits the

activation of a moving reference frame with a steady speed. If the speed is not constant, the transformed

equations will contain additional terms (see Relative Velocity Formulation in the Theory Guide). It should

also be noted that you can run an unsteady simulation in a moving reference frame with constant

speed. This would be necessary if you wanted to simulate, for example, vortex shedding from a rotating

fan blade. The unsteadiness in this case is due to a natural fluid instability (vortex generation) rather

than induced from interaction with a stationary component.

For more information about the equations for moving reference frames, see Equations for a Moving

Reference Frame in the Theory Guide.

Figure . : Single Component (Blower Wheel Blade Passage)

Figure . : Multiple Component (Blower Wheel and Casing)

Modeling Flows with Moving Reference Frames

Many problems permit the entire computational domain to be referred to a single moving reference

frame (hence the name SRF modeling). In such cases, the equations given in Equations for a Moving

Reference Frame are solved in all fluid cell zones. Steady-state solutions are possible in SRF models

provided suitable boundary conditions are prescribed. In particular, wall boundaries must adhere to

the following requirements:

Any walls that are moving with the reference frame can assume any shape. An example would be the blade

surfaces associated with a pump impeller.The no slip condition is defined in the relative frame such that

the relative velocity is zero on the moving walls.

For a rotating problem, you can define walls that are non-moving with respect to the stationary coordinate

system, but these walls must be surfaces of revolution about the axis of rotation. Here the no slip condition

is defined such that the absolute velocity is zero on the walls. An example of this type of boundary would

be a cylindrical wind tunnel wall that surrounds a rotating propeller.

Rotationally periodic boundaries may also be used, but the surface must be periodic about the axis of

rotation. As an example, it is very common to model flow through a blade row of a turbomachine by

assuming the flow to be rotationally periodic and using a periodic domain about a single blade. This

permits good resolution of the flow around the blade without the expense of modeling all blades in

the blade row (see Figure . : Single Blade Model with Rotationally Periodic Boundaries (p. )).

Flow boundary conditions in ANSYS Fluent (inlets and outlets) can, in most cases, be prescribed in either

the stationary or moving frames. For example, for a velocity inlet, one can specify either the relative

velocity or absolute velocity, depending on which is more convenient. For additional information on

these and other boundary conditions, see Setting Up a Single Moving Reference Frame Problem (p. )

and Cell Zone and Boundary Conditions (p. ).

Figure . : Single Blade Model with Rotationally Periodic Boundaries

... Mesh Setup for a Single Moving Reference Frame

It is important to remember the following coordinate-system constraints when you are setting up a

problem involving a moving reference frame for a rotating problem:

For 2D problems, the axis of rotation must be parallel to the  axis.

Flow in Single Moving Reference Frames (SRF)

For 2D axisymmetric problems, the axis of rotation must be the  axis.

For 3D geometries, you should generate the mesh with a specific origin and rotational axis in mind for the

rotating cell zone. Usually it is convenient to use the origin of the global coordinate system (,,) for the

frame origin, and either the ,

, or  axis for the rotational axis; however, ANSYS Fluent can accommodate

an arbitrary origin and rotational axis.

With 3D rotating problems, it is also important to note that if you want to include walls that have zero

velocity in the stationary frame, these walls must be a surface of revolution with respect to the axis

of rotation. If the stationary walls are not surfaces of revolution, you must encapsulate the rotating

parts with interface boundaries, thereby breaking your model up into multiple zones, and use either

the MRF or mixing plane models for steady-state solutions (see The Multiple Reference Frame Mod-

el (p. ) and The Mixing Plane Model (p. )), or the sliding mesh model for unsteady interaction

(see Modeling Flows Using Sliding and Dynamic Meshes (p. )).

... Setting Up a Single Moving Reference Frame Problem

To model a problem involving a single moving reference frame, follow the steps outlined below.

. Select the Velocity Formulation to be used when solving: either Relative or Absolute. (See Choosing

the Relative or Absolute Velocity Formulation (p. ) for details.)

Setup →

General

(Note that this step is irrelevant if you are using one of the density-based solvers; these solvers always

use an absolute velocity formulation.)

. For each cell zone in the domain, specify the translational velocity of the reference frame and/or the an-

gular velocity (

) of the reference frame and the axis about which it rotates.

Setup →

a.

In the Fluid or Solid dialog box, specify the Rotation-Axis Origin and Rotation-Axis Direction for

the frame motion in the Reference Frame tab, in order to define the axis of rotation.

b. Also in the Fluid (Figure . :The Fluid Dialog Box Displaying Frame Motion Inputs (p. )) or Solid

dialog box, enable the Frame Motion option and then set the Speed under Rotational Velocity

and/or the X, Y, and Z components of the Translational Velocity in the expanded portion of the

dialog box under the Reference Frame tab. Note that the speed can be specified as a constant value

or a transient profile.The transient profile may be in a file format, as described in Defining Transient

Cell Zone and Boundary Conditions (p. ), or a UDF macro, described in DEFINE_TRANSIENT_PRO-

FILE. Specifying the individual velocities as either a profile or a UDF allows you to specify a specific

input of the frame motion individually. However, you can also specify the frame motion inputs via a

single user-defined function that uses the UDF macro DEFINE_ZONE_MOTION.This may prove to

be quite convenient if you are modeling a more complicated motion of the moving reference frame,

where the hooking of many different user-defined functions or profiles can be cumbersome.

Note

If you decide to hook a UDF, you will no longer have access to the rotation axis origin

and direction, or the velocities.

Details about these inputs are presented in Inputs for Fluid Zones (p. ) and in Inputs for

Solid Zones (p. ). Details about the zone motion UDF can be found in DEFINE_ZONE_MOTION

in the Fluent Customization Manual.

c.

If you need to switch between the moving reference frame and moving mesh models, simply click

the Copy To Mesh Motion for zones with a moving frame of reference and Copy to Frame Motion

for zones with moving meshes to transfer motion variables, such as the axes, frame origin, and velocity

components between the two models.The variables used for the origin, axis, and velocity components,

as well as for the UDF DEFINE_ZONE_MOTION will be copied.This is particularly useful if you are

doing a steady-state MRF simulation to obtain an initial solution for a transient Moving Mesh simulation

in a turbomachine.

Figure . : The Fluid Dialog Box Displaying Frame Motion Inputs

Important

Normally it is not necessary to enable the Frame Motion option for solid zones, as this

is not required if you want to do a conjugate heat transfer problem where the solid and

fluid zones are moving together. The cases in which you would want to enable the

Frame Motion option include the following:

if you intend to include the convective terms in the energy equation for the solid (see

Equation . in the Theory Guide)

if you are running an intrinsic fluid-structure-interaction (FSI) simulation, and you want the

structural model to account for rotational forces when calculating the deformation of the

solid cell zone (see Modeling Fluid-Structure Interaction (FSI) Within Fluent (p. ))

. Define the velocity boundary conditions at walls.You can choose to define either an absolute velocity or

a velocity relative to the moving reference frame (that is, relative to the velocity of the adjacent cell zone

specified in step ).

If the wall is moving at the speed of the moving frame (and hence stationary in the moving frame),

it is convenient to specify a relative angular velocity of zero. Likewise, a wall that is stationary in

the non-moving frame of reference should be given a velocity of zero in the absolute reference

frame. Specifying the wall velocities in this manner obviates the need to modify these inputs later

if a change is made in the velocity of the fluid zone.

Details about these inputs are presented in Velocity Conditions for Moving Walls (p. ).

. Define the boundary conditions at the inlets, as described in Boundary Conditions (p. ). For velocity

inlets, you can choose to define either absolute velocities or velocities relative to the motion of the adjacent

cell zone (specified in step ). Likewise, the total pressure and flow direction can be prescribed in absolute

or relative frames for pressure inlets.

Details about these inputs are presented in Defining the Flow Direction (p. ) and Defining the

Velocity (p. ).

.... Choosing the Relative or Absolute Velocity Formulation

It is recommended that you use the velocity formulation that will result in most of the flow domain

having the smallest velocities in that frame, thereby reducing the numerical diffusion in the solution

and leading to a more accurate solution.

The absolute velocity formulation is preferred in applications where the flow in most of the domain

is not moving (for example, a fan in a large room). The relative velocity formulation is appropriate

when most of the fluid in the domain is moving, as in the case of a large impeller in a mixing tank.

A problem with stationary outer walls and a rotating impeller can be solved in a single reference

frame. The example is illustrated in Figure . : Geometry with the Rotating Impeller (p. ).

Figure . : Geometry with the Rotating Impeller

In case A, it is expected that only the flow near the impeller would be rotating and that much of

the flow away from the impeller would have a low velocity magnitude in the absolute frame.

Therefore, solving using the absolute velocity formulation is recommended. In case B, most of the

flow is expected to be rotating with a velocity close to that of the impeller. Hence, the relative velocity

formulation is appropriate.

In a situation between case A and case B, either of the formulations may be used.

Important

If the velocity formulation is switched during the solution process, ANSYS Fluent will not

Important

transform the current solution to the other frame, which can lead to large jumps in residuals.

If changing the frame is necessary, it is recommended that you first reinitialize, and then solve.

When one of the density-based solution algorithms is used, the absolute formulation is always

used; the relative velocity formulation is not available in the density-based solvers.

For velocity inlets, pressure inlets, mass-flow inlets, and walls, you may specify velocity in either the

absolute or the relative frame, regardless of whether the absolute or relative velocity formulation is

used in the computation.

For pressure outlets, the specified static pressure is independent of frame. However, when there is

backflow at a pressure outlet, the specified static pressure is used as the total pressure. For calculations

using the absolute velocity formulation, the specified static pressure is used as the total pressure in

the absolute frame; for the relative velocity formulation, the specified static pressure is assumed to

be the total pressure in the relative frame. As for the flow direction, ANSYS Fluent assumes the ab-

solute velocity to be normal to the pressure outlet for the absolute velocity formulation; for the rel-

ative velocity formulation, it is the relative velocity that is assumed to be normal to the pressure

outlet.

... Solution Strategies for a Single Moving Reference Frame

The difficulties associated with solving flows in moving reference frames are similar to those discussed

in Solution Strategies for Axisymmetric Swirling Flows (p. ). The primary issue you must confront is

the high degree of coupling between the momentum equations when the influence of the rotational

terms is large. A high degree of rotation introduces a large radial pressure gradient that drives the

flow in the axial and radial directions, thereby setting up a distribution of the swirl or rotation in the

field. This coupling may lead to instabilities in the solution process, and hence require special solution

techniques to obtain a converged solution. Some techniques that may be beneficial include the follow-

ing:

(Pressure-based solver only) Consider switching the frame in which velocities are solved by changing the

velocity formulation setting in the General Task Page (p. ). (See Choosing the Relative or Absolute Velocity

Formulation (p. ) for details.)

(Pressure-based segregated solver only) Use the PRESTO! scheme (enabled in the Solution Methods Task

Page (p. )), which is well-suited for the steep pressure gradients involved in rotating flows.

(Pressure-based, segregated solver only) Reduce the under-relaxation factors for the velocities, perhaps to

.–. or lower, if necessary.

Begin the calculations using a low rotational speed, increasing the rotational speed gradually in order to

reach the final desired operating condition.

.... Gradual Increase of the Rotational Speed to Improve Solution Stability

Because the rotation of the reference frame and the rotation defined via boundary conditions can

lead to large complex forces in the flow, your ANSYS Fluent calculations may be less stable as the

speed of rotation (and hence the magnitude of these forces) increases. One of the most effective

controls you can exert on the solution is to start with a low rotational speed and then slowly increase

the rotation up to the desired level. The procedure you use to accomplish this is as follows:

. Set up the problem using a low rotational speed in your inputs for boundary conditions and for the an-

gular velocity of the reference frame.The rotational speed in this first attempt might be selected as %

of the actual operating condition.

. Solve the problem at these conditions.

. Modify your inputs (that is, boundary conditions and angular velocity of the reference frame). Increase

the speed of rotation, perhaps doubling it.

. Restart or continue the calculation using the solution data saved in Step  as the initial guess for the

new calculation. Save the new data.

. Continue to increment the rotational speed, following Steps  and , until you reach the desired operating

... Postprocessing for a Single Moving Reference Frame

When you solve a problem in a moving reference frame, you can plot or report both absolute and re-

lative velocities. For all velocity parameters (for example, Velocity Magnitude and Mach Number),

corresponding relative values will be available for postprocessing (for example, Relative Velocity

Magnitude and Relative Mach Number). These variables are contained in the Velocity... category of

the variable selection drop-down list that appears in postprocessing dialog boxes. Relative values are

also available for postprocessing of total pressure, total temperature, and any other parameters that

include a dynamic contribution dependent on the reference frame (for example, Relative Total Pressure,

Relative Total Temperature, Rothalpy).

When plotting velocity vectors, you can choose to plot vectors in the absolute frame (the default), or

you can select Relative Velocity in the Vectors of drop-down list in the Vectors Dialog Box (p. )

to plot vectors in the moving frame. If you plot relative velocity vectors, you might want to color the

vectors by relative velocity magnitude (by choosing Relative Velocity Magnitude in the Color by

list); by default they will be colored by absolute velocity magnitude. Figure . : Absolute Velocity

Vectors (p. ) and Figure . : Relative Velocity Vectors (p. ) show absolute and relative velocity

vectors in a moving domain with a stationary outer wall.

Figure . : Absolute Velocity Vectors

Figure . : Relative Velocity Vectors

Many problems involve multiple moving parts or contain stationary surfaces which are not surfaces of

revolution (and therefore cannot be used with the Single Reference Frame modeling approach). For

these problems, you must break up the model into multiple fluid/solid cell zones, with interface

boundaries separating the zones. Zones that contain the moving components can then be solved using

the moving reference frame equations (Equations for a Moving Reference Frame in the Theory Guide),

whereas stationary zones can be solved with the stationary frame equations. The manner in which the

equations are treated at the interface lead to two approaches that are supported in ANSYS Fluent:

Multiple Moving Reference Frames

– Multiple Reference Frame Model (MRF)

– Mixing Plane Model (MPM)

Sliding Mesh Model (SMM)

Both the MRF and mixing plane approaches are steady-state approximations, and differ primarily in the

manner in which conditions at the interfaces are treated. These approaches will be discussed in the

sections below. The sliding mesh model approach is, on the other hand, inherently unsteady due to

the motion of the mesh with time. This approach is discussed in Modeling Flows Using Sliding and

Dynamic Meshes (p. ).

...The Multiple Reference Frame Model

...The Mixing Plane Model

... Mesh Setup for a Multiple Moving Reference Frame

... Setting Up a Multiple Moving Reference Frame Problem

... Solution Strategies for MRF and Mixing Plane Problems

... Postprocessing for MRF and Mixing Plane Problems

... Frozen Gust / Inlet Disturbance Flow Modeling

Additional information about the MRF model is presented in the following sections:

The MRF model  [] (p. ) is, perhaps, the simplest of the two approaches for multiple zones. It is

a steady-state approximation in which individual cell zones can be assigned different rotational and/or

translational speeds. The flow in each moving cell zone is solved using the moving reference frame

equations (see Introduction (p. )). If the zone is stationary (

), the equations reduce to their

stationary forms. At the interfaces between cell zones, a local reference frame transformation is per-

formed to enable flow variables in one zone to be used to calculate fluxes at the boundary of the

adjacent zone. For more information about the MRF interface formulation, see The MRF Interface

Formulation in the Theory Guide.

It should be noted that the MRF approach does not account for the relative motion of a moving zone

with respect to adjacent zones (which may be moving or stationary); the mesh remains fixed for the

computation. This is analogous to freezing the motion of the moving part in a specific position and

observing the instantaneous flowfield with the rotor in that position. Hence, the MRF is often referred

to as the “frozen rotor approach.”

While the MRF approach is clearly an approximation, it can provide a reasonable model of the flow

for many applications. For example, the MRF model can be used for turbomachinery applications in

which rotor-stator interaction is relatively weak, and the flow is relatively uncomplicated at the interface

between the moving and stationary zones. In mixing tanks, for example, since the impeller-baffle in-

teractions are relatively weak, large-scale transient effects are not present and the MRF model can

be used.

Another potential use of the MRF model is to compute a flow field that can be used as an initial

condition for a transient sliding mesh calculation. This eliminates the need for a startup calculation.

The multiple reference frame model should not be used, however, if it is necessary to actually simulate

the transients that may occur in strong rotor-stator interactions, the sliding mesh model alone should

be used (see Modeling Flows Using Sliding and Dynamic Meshes (p. ).

For more information about and examples of multiple moving reference frames, see The Multiple

Reference Frame Model in the Theory Guide.

The following limitations exist when using the MRF approach:

The interfaces separating a moving region from adjacent regions must be oriented such that the component

of the frame velocity normal to the boundary is zero.This means that for a translationally moving frame,

the moving zone’s boundaries must be parallel to the translational velocity vector. For rotating problems,

the interfaces must be surfaces of revolution about the axis of rotation defined for the fluid zone. For the

Flow in Multiple Moving Reference Frames

example shown Figure . : Geometry with One Rotating Impeller (in the Theory Guide), this requires the

dashed boundary to be circular (not square or any other shape).

Strictly speaking, the use of multiple reference frames is meaningful only for steady flow. However, ANSYS

Fluent will allow you to solve an unsteady flow when multiple reference frames are being used. In this

case, unsteady terms (as described in Temporal Discretization in the Theory Guide) are added to all the

governing transport equations.You should carefully consider whether this will yield meaningful results

for your application, because, for unsteady flows, a sliding mesh calculation will generally yield more

meaningful results than an MRF calculation.

By default, pathlines and particle trajectories drawn by ANSYS Fluent use the velocity relative to the refer-

ence frame motion of the cell zone. However, for particle trajectories, you can change the reference frame

by either selecting Track in Absolute Frame in the Numerics tab of the Discrete Phase Model dialog

box or using the text command define/models/dpm/options/track-in-absolute-frame.

Note

Only the default behavior (tracking relative to the moving reference frame) ensures that

pathlines and massless particles follow the flow in a physically reasonable way; that is,

pathlines or massless particles will not hit a wall surface with any strong wall-normal

velocity component. Consistently with this, when a pathline or particle trajectory crosses

a boundary between zones with different reference frame motion specifications, you

may observe a sharp change in particle velocity as a result of the coordinate transform-

ation.

The particle injection velocities (specified in the Set Injection Properties Dialog Box (p. )) are in-

terpreted in the same way as tracking, that is, either relative to the local frame of reference’s motion

specification or in absolute coordinates.

You cannot accurately model axisymmetric swirl in the presence of multiple reference frames using the

relative velocity formulation.This is because the current implementation does not apply the transformation

used in Equation . (in the Theory Guide) to the swirl velocity derivatives. For this situation, the absolute

velocity formulation should be used.

Translational and rotational velocities are assumed to be constant (time varying

,

are not allowed).

The relative velocity formulation cannot be used in combination with the MRF and mixture models. (For

details, see Mixture Model Theory in the Theory Guide). For such cases, use the absolute velocity formulation

instead.

You must not have a single interface between reference frames where part of the interface is made up of

a coupled two-sided wall, while another part is not coupled (that is, the normal interface treatment). In

such cases, you must break the interface up into two interfaces: one that is a coupled interface, and the

other that is a standard fluid-fluid interface. See Using a Non-Conformal Mesh in ANSYS Fluent (p. ) for

the steps involved in setting up a coupled interface.

Important

You can switch from the MRF model to the sliding mesh model for a more robust and ac-

curate solution, by using the mesh/modify-zones/mrf-to-sliding-mesh text

command. See Using Sliding Meshes (p. ) for details on how to make this change in the

fluid’s boundary conditions.

The mixing plane model in ANSYS Fluent provides an alternative to the multiple reference frame and

sliding mesh models for simulating flow through domains with one or more regions in relative motion.

Additional information about the mixing plane model is presented in the following sections:

As discussed in The Multiple Reference Frame Model (p. ), the MRF model is applicable when the

flow at the interface between adjacent moving/stationary zones is nearly uniform (“mixed out”). If

the flow at this interface is not uniform, the MRF model may not provide a physically meaningful

solution. The sliding mesh model (see Modeling Flows Using Sliding and Dynamic Meshes (p. ))

may be appropriate for such cases, but in many situations it is not practical to employ a sliding mesh.

For example, in a multistage turbomachine, if the number of blades is different for each blade row,

a large number of blade passages is required in order to maintain circumferential periodicity. Moreover,

sliding mesh calculations are necessarily unsteady, and therefore require significantly more computation

to achieve a final, time-periodic solution. For situations where using the sliding mesh model is not

feasible, the mixing plane model can be a cost-effective alternative.

In the mixing plane approach, each fluid zone is treated as a steady-state problem. Flow-field data

from adjacent zones are passed as boundary conditions that are spatially averaged or “mixed” at the

mixing plane interface. This mixing removes any unsteadiness that would arise due to circumferential

variations in the passage-to-passage flow field (for example, wakes, shock waves, separated flow),

therefore yielding a steady-state result. Despite the simplifications inherent in the mixing plane

model, the resulting solutions can provide reasonable approximations of the time-averaged flow field.

Note the following limitations of the mixing plane model:

The LES turbulence model cannot be used with the mixing plane model.

The models for species transport and combustion cannot be used with the mixing plane model.

The VOF multiphase model cannot be used with the mixing plane model.

The discrete phase model cannot be used with the mixing plane model for coupled flows. Non-coupled

computations can be done, but you should note that the particles leave the domain of the mixing plane.

You can find more information about the following topics in the Theory Guide:

Rotor and Stator Domains

The Mixing Plane Concept

Choosing an Averaging Method

Mixing Plane Algorithm of ANSYS Fluent

Mass Conservation

Swirl Conservation

Total Enthalpy Conservation

Two mesh setup methods are available. Choose the method that is appropriate for your model, noting

the restrictions in Limitations (p. ).

If the boundary between two zones that are in different reference frames is conformal (that is, the mesh

node locations are identical at the boundary where the two zones meet), you can simply create the mesh

as usual, with all cell zones contained in the same mesh file. A different cell zone should exist for each

portion of the domain that is modeled in a different reference frame. Use an interior zone for the boundary

between reference frames.

If the boundary between two zones that are in different reference frames is non-conformal (that is, the

mesh node locations are not identical at the boundary where the two zones meet), follow the non-conformal

mesh setup procedure described in Using a Non-Conformal Mesh in ANSYS Fluent (p. ).

To learn more about setting up a multiple reference frame problem, see the following sections:

.... Setting Up Multiple Reference Frames

.... Setting Up the Mixing Plane Model

To model a problem involving multiple reference frames, perform the following:

Important

The mesh-setup constraints for a moving reference frame listed in Mesh Setup for a Single

Moving Reference Frame (p. ) apply to multiple reference frames as well.

. Select the Velocity Formulation to be used in the General Task Page (p. ): either Absolute or Relative.

(For details, see Choosing the Relative or Absolute Velocity Formulation (p. ).)

Setup →

General

(Note that this step is irrelevant if you are using one of the density-based solution algorithms;

these algorithms always use an absolute velocity formulation.)

. For each cell zone in the domain, specify its translational velocity and/or its angular velocity (

) and the

axis about which it rotates.

Setup →

a.

If the zone is moving, or if you plan to specify cylindrical velocity or flow-direction components at

inlets to the zone, you must define the axis of rotation of the frame of reference. In the Fluid or Solid

dialog box, specify the Rotation-Axis Origin and Rotation-Axis Direction under the Reference

Frame tab.

b. In the Fluid (Figure . :The Fluid Dialog Box Displaying Frame Motion Inputs (p. )) or Solid dialog

box, enable the Frame Motion option. Set the Speed under Rotational Velocity and/or the X, Y,

and Z components of the Translational Velocity in the expanded portion of the dialog box under

Note that the speed can be specified as a constant value or a transient profile. The transient

profile may be in a file format, as described in Defining Transient Cell Zone and Boundary

Conditions (p. ), or a UDF macro, described in DEFINE_TRANSIENT_PROFILE. Specifying

the individual velocities as either a profile or a UDF allows you to specify a specific input of

the frame motion individually. However, you can also specify the frame motion inputs via a

single user-defined function that uses the UDF macro DEFINE_ZONE_MOTION. This may

prove to be quite convenient if you are modeling a more complicated motion of the moving

reference frame, where the hooking of many different user-defined functions or profiles can

Note

If you decide to hook a UDF, then you will no longer have access to the rotation

axis origin and direction, or the velocities.

Solid Zones (p. ). Details about the zone motion UDF can be found in DEFINE_ZONE_MO-

TION in the Fluent Customization Manual.

c.

To switch between the MRF and moving mesh models, click the Copy To Mesh Motion for zones

c.

with a moving frame of reference and Copy to Frame Motion for zones with moving meshes to

transfer motion variables, such as the axes, frame origin, and velocity components between the two

models.

The variables used for the origin, axis, and velocity components, as well as for the UDF

DEFINE_ZONE_MOTION will be copied. This is particularly useful if you are doing a steady-

state MRF simulation to obtain an initial solution for a transient Moving Mesh simulation in a

turbomachine.

. Define the velocity boundary conditions at walls.You can choose to define either an absolute velocity

or a velocity relative to the velocity of the adjacent cell zone specified in step .

If the wall is moving at the speed of the moving frame (and hence stationary relative to the

moving frame), it is convenient to specify a relative angular velocity of zero. Likewise, a wall that

is stationary in the non-moving frame of reference should be given a velocity of zero in the absolute

reference frame. Specifying the wall velocities in this manner obviates the need to modify these

inputs later if a change is made in the rotational velocity of the fluid zone.

An example for which you would specify a relative velocity is as follows: If an impeller is defined

as wall- and the fluid region within the impeller’s radius is defined as fluid-, you would need

to specify the angular velocity and axis of rotation for fluid- and then assign wall- a relative

velocity of . If you later wanted to model a different angular velocity for the impeller, you would

need to change only the angular velocity of the fluid region; you would not need to modify the

wall velocity conditions.

inlets, you can choose to define either absolute velocities or velocities relative to the motion of the adja-

cent cell zone (specified in step ). Likewise, the total pressure and flow direction can be prescribed in

absolute or relative frames for pressure inlets.

. Define the mesh interfaces using the Mesh Interfaces Dialog Box (p. ) (Figure . :The Mesh Interfaces

New...

To learn how to use the Mesh Interfaces dialog box, see Using a Non-Conformal Mesh in ANSYS

Fluent (p. ).

. Initialize the solution using an absolute frame of reference (Figure . :The Solution Initialization Task

Page for Moving Reference Frames (p. )).

Solution →

Select the Absolute option under Reference Frame. If the Relative to Cell Zone option is selected,

the initial flow field can contain discontinuities, which can cause convergence problems in the

first few iterations.

Figure . : The Solution Initialization Task Page for Moving Reference Frames

The model inputs for mixing planes are presented in this section. Only those steps relevant specifically

to the setup of a mixing plane problem are listed here. Note that the use of wall and periodic

boundaries in a mixing plane model is consistent with their use when the model is not active.

. Select the Absolute or Relative Velocity Formulation in the General Task Page (p. ), when the

pressure-based solver is enabled.

Setup →

General

Important

When the density-based solver is enabled, only the Absolute Velocity Formulation

can be used with the mixing plane model.

. For each cell zone in the domain, specify its angular velocity (

) and the axis about which it rotates.

Setup →

a.

If the zone is rotating, or if you plan to specify cylindrical-velocity or flow-direction components at

inlets to the zone, you must define the axis of rotation for the frame of reference. In the Fluid dialog

box or Solid Dialog Box (p. ), specify the Rotation-Axis Origin and Rotation-Axis Direction under

box, enable the Frame Motion option and then set the Speed under Rotational Velocity and/or

the X, Y, and Z components of the Translational Velocity in the expanded portion of the dialog box

under the Reference Frame tab.

Important

It is important to define the axis of rotation for the cell zones on both sides of the

mixing plane interface, including the stationary zone.

. Define the velocity boundary conditions at walls, as described in step  of Setting Up Multiple Reference

cent cell zone (specified in step ). For pressure inlets and mass-flow inlets, the specification of the flow

direction and total pressure will always be absolute, because the absolute velocity formulation is always

used for mixing plane calculations. For a mass-flow inlet, you do not need to specify the mass flow rate

or mass flux. ANSYS Fluent will automatically select the Mass Flux with Average Mass Flux specification

method and set the correct values when you create the mixing plane, as described in More About Mass

Flux and Average Mass Flux (p. ).

Details about these inputs are presented in Defining the Flow Direction (p. ), Defining the Ve-

locity (p. ), and Inputs at Mass-Flow Inlet Boundaries (p. ).

Important

Note that the outlet boundary zone at the mixing plane interface must be defined as

a pressure outlet, and the inlet boundary zone at the mixing plane interface must be

defined as either a velocity inlet (incompressible flow only), a pressure inlet, or a mass-

flow inlet. The overall inlet and exit boundary conditions can be any suitable combina-

tion permitted by the solver (for example, velocity inlet, pressure inlet, or mass-flow

inlet; pressure outlet). Remember, however, that if mass conservation across the mixing

plane is important, you must use a mass-flow inlet as the downstream boundary; strict

mass conservation is not maintained across the mixing plane when you use a velocity

inlet or pressure inlet.

. Define the mixing planes in the Mixing Planes Dialog Box (p. ) (Figure . :The Mixing Planes Dialog

Box (p. )).

Domain → Mesh Models → Mixing Planes...

Figure . : The Mixing Planes Dialog Box

a.

Specify the two zones that make up the mixing plane by selecting an upstream zone in the Upstream

Zone list and a downstream zone in the Downstream Zone list. It is essential that the correct pairs

be chosen from these lists (that is, that the boundary zones selected lie on the mixing plane interface).

You can check this by displaying the mesh.

Setup →

b. (3D only) Indicate the geometry of the mixing plane interface by choosing one of the options under

Mixing Plane Geometry.

A Radial geometry signifies that information at the mixing plane interface is to be circumfer-

entially averaged into profiles that vary in the radial direction, for example,

,

. This

is the case for axial-flow machines, for example.

An Axial geometry signifies that circumferentially averaged profiles are to be constructed that

vary in the axial direction, for example,

,

. This is the situation for a radial-flow device.

Important

Note that the radial direction is normal to the rotation axis for the fluid zone and

the axial direction is parallel to the rotation axis.

c.

(3D only) Set the number of Interpolation Points.This is the number of radial or axial locations used

in constructing the boundary profiles for circumferential averaging.You should choose a number

that approximately corresponds to the resolution of the surface mesh in the radial or axial direction.

Note that while you can use more points if you want, the resolution of the boundary profile will only

be as fine as the resolution of the surface mesh itself.

In 2D the flow data is averaged over the entire interface to create a profile consisting of a

single data point. For this reason you do not need to set the number of Interpolation Points

or select a Mixing Plane Geometry in 2D.

d. Set the Global Parameters for the mixing plane.

i.

Select the Averaging Method.The Area averaging method is the default method. For detailed

information about each of the Area, Mass, or Mixed-Out options, see Choosing an Averaging

Method in the Theory Guide.

ii.

Set the Under-Relaxation parameter. It is sometimes desirable to under-relax the changes in

boundary values at mixing planes as these may change very rapidly during the early iterations of

the solution and cause the calculation to diverge.The changes can be relaxed by specifying an

under-relaxation less than .The new boundary profile values are then computed using

(.)

where  is the under-relaxation factor. Once the flow field is established, the value of

can be increased.

iii. Click Apply to set the Global Parameters. If the Default button is visible to the right of the Apply

button, clicking the Default button will return Global Parameters back to their default values.

The Default button will then change to be a Reset button. Clicking the Reset button will change

the Global Parameters back to the values that were last applied.

e. Click Create to create a new mixing plane. ANSYS Fluent will name the mixing plane by combining

the names of the zones selected as the Upstream Zone and Downstream Zone and enter the new

mixing plane in the Mixing Plane list.

If you create an incorrect mixing plane, you can select it in the Mixing Plane list and click the

Delete button to delete it.

..... Modeling Options

There are two options available for use with the mixing plane model: a fixed pressure level for in-

compressible flows, and the swirl conservation described in Swirl Conservation in the Theory Guide.

...... Fixing the Pressure Level for an Incompressible Flow

For certain turbomachinery configurations, such as a torque converter, there is no fixed-pressure

boundary when the mixing plane model is used. The mixing plane model is usually used to model

the three interfaces that connect the components of the torque converter. In this configuration, the

pressure is no longer fixed. As a result, the pressure may float unbounded, making it difficult to

obtain a converged solution.

To resolve this problem, ANSYS Fluent offers an option for fixing the pressure level. When this option

is enabled, ANSYS Fluent will adjust the gauge pressure field after each iteration by subtracting from

it the pressure value in the cell closest to the Reference Pressure Location in the Operating Condi-

tions Dialog Box (p. ).

Important

Important

This option is available only for incompressible flows calculated using the pressure-based

solver.

To enable the fixed pressure option, use the fix-pressure-level text command:

define → mixing-planes → set → fix-pressure-level

...... Conserving Swirl Across the Mixing Plane

Conservation of swirl is important for applications such as torque converters (Swirl Conservation in

the Theory Guide). If you want to enable swirl conservation across the mixing plane, you can use

the commands in the conserve-swirl text menu:

define → mixing-planes → set → conserve-swirl

To turn on swirl conservation, use the enable? text command. Once the option is turned on, you

can ask the solver to report information about the swirl conservation during the calculation. If you

turn on verbosity?, ANSYS Fluent will report for every iteration the zone ID for the zone on which

the swirl conservation is active, the upstream and downstream swirl integration per zone area, and

the ratio of upstream to downstream swirl integration before and after the correction.

To obtain a report of the swirl integration at every pressure inlet, pressure outlet, velocity inlet, and

mass-flow inlet in the domain, use the report-swirl-integration command. You can use

this information to determine the torque acting on each component of the turbomachinery according

to Equation . (in the Theory Guide).

...... Conserving Total Enthalpy Across the Mixing Plane

One of the options available in the mixing plane model is to conserve total enthalpy across the

mixing plane. This is a desirable feature because global parameters such as efficiency are directly

related to the change in total enthalpy across a blade row or stage.

The procedure for ensuring conservation of total enthalpy simply involves adjusting the downstream

total temperature profile such that the integrated total enthalpy matches the upstream integrated

total enthalpy.

If you want to enable total enthalpy conservation, you can use the commands in the conserve-

total-enthalpy text menu:

define → mixing-planes → set → conserve-total-enthalpy

To turn on total enthalpy conservation, use the enable? text command. Once the option is turned

on, you can ask the solver to report information about the total enthalpy conservation during the

calculation. If you turn on verbosity?, ANSYS Fluent will report at every iteration the zone ID for

the zone on which the total enthalpy conservation is active, the upstream and downstream heat

flux, and the ratio of upstream to downstream heat flux.

.... MRF Model

For multiple moving reference frames, follow the guidelines presented in Solution Strategies for a

Single Moving Reference Frame (p. ) for a single moving reference frame. Remember that with

multiple zones, the possibility exists of interaction between moving and stationary components. This

will manifest itself as poor or oscillatory convergence. In such cases, it is strongly recommend that

the sliding mesh approach be used to compute the flowfield in order to resolve the unsteady inter-

actions.

.... Mixing Plane Model

actions.

It should be emphasized that the mixing plane model is a reasonable approximation so long as there

is no significant reverse flow in the vicinity of the mixing plane. If significant reverse flow occurs, the

mixing plane will not be a satisfactory model of the actual flow. In a numerical simulation, reverse

flow often occurs during the early stages of the computation even though the flow at convergence

is not reversed. Therefore, it is helpful in these situations to first obtain a provisional solution using

fixed conditions at the rotor-stator interface. The mixing plane model can then be enabled and the

solution run to convergence.

If you are using the mass or mixed-out averaging method and you are experiencing convergence

problems in the presence of severe reverse flow, initialize your solution using the default area-averaging

method, then switch to mass or mixed-out averaging after the reverse flow dies out.

Under-relaxing the changes in the mixing plane boundary values can also help in troublesome situ-

ations. In many cases, setting the under-relaxation factor to a value less than  can be helpful. Once

the flow field is established, you can gradually increase the under-relaxation factor.

When you solve a problem using the multiple reference frame or mixing plane model, you can plot

or report both absolute and relative velocities. For all velocity parameters (for example, Velocity

Magnitude and Mach Number), corresponding relative values will be available for postprocessing

(for example, Relative Velocity Magnitude and Relative Mach Number). These variables are contained

in the Velocity... category of the variable selection drop-down list that appears in postprocessing

dialog boxes. Relative values are also available for postprocessing of total pressure, total temperature,

and any other parameters that include a dynamic contribution dependent on the reference frame (for

example, Relative Total Pressure, Relative Total Temperature).

Important

Relative velocities are relative to the translational/rotational velocity of the “reference zone”

(specified in the Reference Values task page (see Reference Values Task Page (p. ))). The

velocity of the reference zone is the velocity defined in the Fluid Dialog Box (p. ) for that

zone.

to plot vectors relative to the translational/rotational velocity of the “reference zone” (specified in the

Reference Values Task Page (p. )). If you plot relative velocity vectors, you might want to color the

list); by default they will be colored by absolute velocity magnitude.

You can also generate a plot of circumferential averages in ANSYS Fluent. This allows you to find the

average value of a quantity at several different radial or axial positions in your model. ANSYS Fluent com-

putes the average of the quantity over a specified circumferential area, and then plots the average

against the radial or axial coordinate. For more information on generating XY plots of circumferential

averages, see XY Plots of Circumferential Averages (p. ).

For details about turbomachinery-specific postprocessing features see Turbomachinery Postpro-

cessing (p. ).

To reduce blade row simulation cost in turbomachinery you can model blade row coupling (rotor /

stator interaction) using a technique known as frozen gust or inlet disturbance flow modeling. In this

modeling strategy, the wake of the upstream row is obtained usually from a steady-state simulation

and imposed as an inlet profile on the downstream blade row. The same can be done with the potential

field from the downstream row on an upstream row. By doing this, the blade row interaction problem

is reduced to a single row with imposed inlet and/or outlet profiles.

There are two possible variations of this flow problem. See Figure . : Frozen Gust variations (p. ).

Wake from a rotor imposed on stator row (configuration A).

Wake from a stator imposed on rotor row (configuration B).

Figure . : Frozen Gust variations

The common workflow for the frozen gust / inlet disturbance modeling approach is as follows:

. Perform a steady-state simulation of the blade row interactions for the rotor / stator configuration of interest

using either the mixing plane or frozen-rotor method. See The Multiple Reference Frame Model (p. )

or The Mixing Plane Model (p. ).

. Extract the wake profile from the neighboring row (wake of the upstream row or potential field of the

downstream row). See Reading and Writing Profile Files (p. ).

. Expand the wake profile to full wheel using the Replicate Profile dialog box. See Replicating Profiles (p. ).

. Apply the expanded profile to the boundary of interest, typically an inlet, on the rotor or stator depending

on the configuration.

. The final step is dependent on which configuration you are modeling.

For rotor wake imposed on stator passage (configuration A):

The profile must be linked to a reference frame that is rotating with the rotor. See Using Pro-

files (p. ).

For stator wake imposed on a rotor passage (configuration B):

The motion of the rotor with respect to the stationary stator wake profile can be modeled using

the standard Mesh Motion feature in Fluent, where the rotation of the rotor and the axis of rotation

are specified in the fluid cell zone conditions. See Defining Zone Motion (p. ).

Chapter : Modeling Flows Using Sliding and Dynamic Meshes

This chapter describes the setup and use of the sliding and dynamic mesh models in ANSYS Fluent. To

learn more about the theory of sliding meshes in ANSYS Fluent, see Sliding Mesh Theory in the Theory

Guide. For more information about the theory behind dynamic meshes in ANSYS Fluent, see Dynamic

Mesh Theory in the Theory Guide.

Understanding and using the sliding and deforming mesh models is presented in the following sections:

.. Sliding Mesh Examples

..The Sliding Mesh Technique

.. Sliding Mesh Interface Shapes

.. Using Sliding Meshes

.. Using Dynamic Meshes

The sliding mesh model allows you to set up a problem in which separate zones move relative to each

other. The motion can be translational or rotational. The relative motion of stationary and moving

components (for example, in a rotating machine) will give rise to transient interactions. Often, the

transient solution that is sought in a sliding mesh simulation is time-periodic. That is, the transient

solution repeats with a period related to the speeds of the moving domains.

The dynamic mesh model allows you to move the boundaries of a cell zone relative to other boundaries

of the zone, and to adjust the mesh accordingly. The boundaries can move rigidly with respect to each

other (that is, linear or rotational motion), and/or deform.

When deciding whether to use a sliding mesh versus a dynamic mesh, consider the following:

Many problems could be solved by either approach.

If the problem does not involve mesh deformation, the sliding mesh model is recommended, as it is

simpler and more efficient.

The dynamic mesh method must be used if the mesh is deforming, or if the mesh motion is a function

of the solution (for example, the six degrees of freedom solver).

Important

Sliding mesh and dynamic mesh are incompatible if they are combined within the same cell

zone or adjacent cell zones. If you want to combine these two models within the same case

file, they must be separated by a non-moving cell zone.

Note

Note

By default, transient simulations that involve a rotating fluid zone utilize a better flow field

predictor that can speed up the calculation in some flow simulations. You can deactivate

the flow field predictor by using the command solve/set/rotating-mesh-flow-

predictor? and answering no.

For examples of typical sliding mesh and dynamic mesh problems, see Introduction in the Theory Guide.

When a time-accurate solution (rather than a time-averaged solution) for rotor-stator interaction is desired,

you must use the sliding mesh model to compute the unsteady flow field. The sliding mesh model is

the most accurate method for simulating flows in multiple moving reference frames, but also the most

computationally demanding.

Most often, the unsteady solution that is sought in a sliding mesh simulation is time-periodic. That is,

the unsteady solution repeats with a period related to the speeds of the moving domains. However,

you can model other types of transients, including translating sliding mesh zones (for example, two

cars or trains passing in a tunnel, as shown in Figure . : Two Passing Trains in a Tunnel (p. )). Note

that the sliding mesh can be modeled using periodic boundaries (Figure . : Rotor-Stator Interaction

(Stationary Guide Vanes with Rotating Blades) (p. )) or a circular/cylindrical interface (Fig-

ure . : Blower (p. )).

Figure . : Two Passing Trains in a Tunnel

Modeling Flows Using Sliding and Dynamic Meshes

Figure . : Rotor-Stator Interaction (Stationary Guide Vanes with Rotating Blades)

Figure . : Blower

Note that for flow situations where there is no interaction between stationary and moving parts (for

example, when there is only a rotor), it is not necessary to use a sliding mesh, and the moving reference

frame model is recommended. (See Flow in a Moving Reference Frame for details.) If you are interested

in a steady approximation of the interaction, you may use the multiple reference frame model or the

mixing plane model, as described in The Multiple Reference Frame Model and The Mixing Plane Model

Sliding Mesh Examples

In the sliding mesh technique, two or more cell zones are used. (If you generate the mesh in each zone

independently, you must merge the mesh files prior to starting the calculation, as described in Reading

Multiple Mesh/Case/Data Files (p. ) in the User’s Guide.) Each cell zone is bounded by at least one

“interface zone” where it meets the opposing cell zone. The interface zones of adjacent cell zones are

associated with one another to form a “mesh interface.” The two cell zones will move relative to each

other along the mesh interface.

During the calculation, the cell zones slide (that is, rotate or translate) relative to one another along the

mesh interface in discrete steps. Figure . : Initial Position of the Meshes (p. ) and Figure . : Rotor

Mesh Slides with Respect to the Stator (p. ) show the initial position of two meshes and their positions

after some translation has occurred. Note that all non-conformal interfaces will be automatically updated

(if necessary) by ANSYS Fluent when the mesh is updated.

As the rotation or translation takes place, node alignment along the mesh interface is not required.

Since the flow is inherently unsteady, a time-dependent solution procedure is required.

Figure . : Initial Position of the Meshes

Figure . : Rotor Mesh Slides with Respect to the Stator

The mesh interface and the associated interface zones can be any shape, provided that the two interface

boundaries are based on the same geometry. Figure . : 2D Linear Mesh Interface (p. ) shows an

example with a linear mesh interface and Figure . : 2D Circular-Arc Mesh Interface (p. ) shows a

circular-arc mesh interface. (In both figures, the mesh interface is designated by a dashed line.)

Figure . : 2D Linear Mesh Interface

Sliding Mesh Interface Shapes

Figure . : 2D Circular-Arc Mesh Interface

If Figure . : 2D Linear Mesh Interface (p. ) was extruded to 3D, the resulting sliding interface would

be a planar rectangle; if Figure . : 2D Circular-Arc Mesh Interface (p. ) was extruded to 3D, the

resulting interface would be a cylinder. Figure . : 3D Conical Mesh Interface (p. ) shows an example

that would use a conical mesh interface. (The slanted, dashed lines represent the intersection of the

conical interface with a 2D plane.)

Figure . : 3D Conical Mesh Interface

For an axial rotor/stator configuration, in which the rotating and stationary parts are aligned axially instead

of being concentric (see Figure . : 3D Planar-Sector Mesh Interface (p. )), the interface will be a

planar sector. This planar sector is a cross-section of the domain perpendicular to the axis of rotation

at a position along the axis between the rotor and the stator.

Figure . : 3D Planar-Sector Mesh Interface

This section describes how to use sliding meshes, including restrictions and constraints, problem setup,

solution strategies, and postprocessing.

... Requirements, Constraints, and Considerations

... Setting Up the Sliding Mesh Problem

... Solution Strategies for Sliding Meshes

... Postprocessing for Sliding Meshes

Before beginning the problem setup in ANSYS Fluent, be sure that the mesh you have created meets

The mesh must have a different cell zone for each portion of the domain that is sliding at a different speed.

The mesh interface must be situated such that there is no motion normal to it.

The mesh interface can be any shape (including a non-planar surface, in 3D), provided that the two interface

boundaries are based on the same geometry. If there are sharp features in the mesh (for example, -degree

angles), it is especially important that both sides of the interface closely follow that feature.

If you create a single mesh with multiple cell zones, you must be sure that each cell zone has a distinct face

zone on the sliding boundary.The face zones for two adjacent cell zones will have the same position and

shape, but one will correspond to one cell zone and one to the other. (Note that it is also possible to create

a separate mesh file for each of the cell zones, and then merge them as described in Reading Multiple

Mesh/Case/Data Files (p. ).)

Using Sliding Meshes

If you are modeling a rotor/stator geometry using periodicity, the periodic angle of the mesh around the

rotor blade(s) must be the same as that of the mesh around the stationary vane(s).

All periodic zones must be correctly oriented (either rotational or translational) before you create the mesh

Note the following limitations if you want to use the periodic repeats option as part of the mesh interface:

– The edges of the second interface zone must be offset from the corresponding edges of the first interface

zone by a uniform amount (either a uniform translational displacement or a uniform rotation angle).

– Some portion of the two interface zones must overlap (that is, be spatially coincident).

– The non-overlapping portions of the interface zones must have identical shape and dimensions at all

times during the mesh motion.

– One pair of conformal periodic zones must be adjacent to each of the interface zones. For example, when

you calculate just one channel and blade of a fan, turbine, and so on, you must have conformal periodics

on either side of the interface threads.This will not work with non-conformal periodics.

Note that for 3D cases, you cannot have more than one pair of conformal periodic zones adjacent

to each of the interface zones.

You must not have a single sliding mesh interface where part of the interface is made up of a coupled two-

sided wall, while another part is not coupled (that is, the normal interface treatment). In such cases, you

must break the interface up into two interfaces: one that is a coupled interface, and the other that is a

standard fluid-fluid interface. See Using a Non-Conformal Mesh in ANSYS Fluent (p. ) for information

When using the sliding mesh technique, mass fluxes are interpolated from the sliding interface faces to

the sliding boundary faces, which can affect the local mass balance at the sliding boundary.This can result

in pressure field oscillations at the sliding boundary.These oscillations may be reduced by ensuring the

surface mesh node distributions are similar on either side of the sliding boundaries.You can use the

matching option (Matching Option (p. )), where applicable, to reduce solution oscillations at the sliding

For details about these restrictions and general information about how the sliding mesh model works

in ANSYS Fluent, see The Sliding Mesh Technique (p. ).

The steps for setting up a sliding mesh problem are listed below. (Note that this procedure includes

only those steps necessary for the sliding mesh model itself; you must set up other models, boundary

conditions, and so on, as usual.)

. Enable the appropriate option for modeling transient flow. (See Performing Time-Dependent Calcula-

tions (p. ) for details about the transient modeling capabilities in ANSYS Fluent.)

Analysis Type → Transient

. Set the cell zone conditions for the sliding motion:

Setup →

In the Solid Dialog Box (p. ) or Fluid Dialog Box (p. ) of each moving fluid or solid zone, enable

Setup →

the Mesh Motion option and set the translational and/or rotational velocity under the Mesh Motion

tab. (Note that a solid zone cannot move at a different speed than an adjacent fluid zone.)

Important

Note that simultaneous translation and rotation can be modeled only if the rotation

axis and the translation direction are the same (that is, the origin is fixed).

Note that the speed can be specified as a constant value or a transient profile. The transient profile

may be in a file format, as described in Defining Transient Cell Zone and Boundary Conditions (p. ),

or a UDF macro, described in DEFINE_TRANSIENT_PROFILE in the Fluent Customization

Manual. Specifying the individual velocities as either a profile or a UDF allows you to specify a

single component of the frame motion individually. However, you can also specify the frame motion

using a user-defined function. This may prove to be quite convenient if you are modeling a more

complicated motion of the moving reference frame, where the hooking of many different user-

defined functions or profiles can be cumbersome.

Note

. Set the boundary conditions for the sliding motion:

Setup →

Change the zone Type of the interface zones of adjacent cell zones to interface in the Boundary

Conditions Task Page (p. ).

By default, the velocity of a wall is set to zero relative to the motion of the adjacent mesh. For walls

bounding a moving mesh this results in a “no-slip” condition in the reference frame of the mesh.

Therefore, you need not modify the wall velocity boundary conditions unless the wall is stationary

in the absolute frame, and therefore moving in the relative frame. See Velocity Conditions for

Moving Walls (p. ) for details about wall motion.

See Cell Zone and Boundary Conditions (p. ) for details about inputting cell zone and boundary

New...

Fluent (p. ). Note that the Interface Options that are relevant for sliding meshes are Periodic

Repeats, Coupled Wall, and Matching (for more information on these options, see Non-Conformal

Mesh Calculations (p. )).

. Preview the mesh motion using the Zone Motion dialog box, which can be opened from the Run Calcu-

lation task page.

Solution → Run Calculation

Preview Mesh Motion...

For details about using the Zone Motion dialog box, see Previewing the Dynamic Mesh (p. ).

Important

When you have completed the problem setup, you should save an initial case file so that

you can easily return to the original mesh position (that is, the positions before any sliding

occurs). The mesh position is stored in the case file, so case files that you save at different

times during the transient calculation will contain meshes at different positions.

Important

Important

If you want to go from an MRF model setup to a sliding mesh setup, use the following text

command:

mesh → modify-zones → mrf-to-sliding-mesh

To successfully switch from an MRF to a sliding mesh, you must provide the ID of the fluid

zone. ANSYS Fluent identifies all the zones belonging to this fluid zone, as well as fluid

zones shared in the domain. ANSYS Fluent then splits these zones into walls, after which

the walls are slit converted to interfaces. ANSYS Fluent then changes the cell zone condition

of the fluid zone to Moving Mesh in the Fluid Dialog Box (p. ). Note that the interface

between the cells zones should be an interior boundary. You do not need to do this if you

have already created a mesh interface. The sliding mesh solution tends to be more robust

than the MRF solution.

You will begin the sliding mesh calculation by initializing the solution (as described in Initializing the

Entire Flow Field Using Standard Initialization (p. )) and then specifying the time step size and

number of time steps in the Run Calculation Task Page (p. ), as for any other transient calculation.

(See Performing Time-Dependent Calculations (p. ) for details about time-dependent solutions.)

Note that the time step size in the initial case file is saved without clicking Calculate. ANSYS Fluent will

iterate on the current time step solution until satisfactory residual reduction is achieved, or the max-

imum number of iterations per time step is reached. When it advances to the next time step, the cell

and wall zones will automatically be moved according to the specified translational or rotational velo-

cities (as discussed in the previous section). The new interface-zone intersections will be computed

automatically, and resultant interior/periodic/external boundary zones will be updated.

Note that you can run the MRF case using mesh interfaces with an appreciable loss of accuracy, doing

so makes it easier to later on convert to a sliding mesh.

Note

The sliding mesh can be initialized with an MRF solution (rather using Standard or Hybrid

initializations).

It is recommended that you preview the sliding mesh motion (as described in Previewing the Dynamic

Mesh (p. )) before beginning your calculation. This can catch problems with the motion specification(s)

before you begin the CFD calculation. Remember to save the case and initial data files before doing

a mesh preview since the mesh position is altered once you do the preview. You can reread the initial

condition case/data files to get back to the original mesh position.

.... Saving Case and Data Files

ANSYS Fluent’s automatic saving of case and data files (see Automatic Saving of Case and Data

Files (p. )) can be used with the sliding mesh model. This provides a convenient way for you to

save results at successive time steps for later postprocessing.

Important

You must save a case file each time you save a data file because the mesh position is

stored in the case file. Since the mesh position changes with each time step, reading data

Important

for a given time step will require the case file at that time step so that the mesh will be

in the proper position. You should also save your initial case file so that you can easily return

to the mesh’s original position to restart the solution if desired.

....Time-Periodic Solutions

For some problems (for example, rotor-stator interactions), you may be interested in a time-periodic

solution. That is, the startup transient behavior may not be of interest to you. Once this startup phase

has passed, the flow will start to exhibit time-periodic behavior. If

is the period of unsteadiness,

then for some flow property

at a given point in the flow field:

(.)

For rotating problems, the period (in seconds) can be calculated by dividing the sector angle of the

domain (in radians) by the rotor speed (in radians/sec):

. For 2D rotor-stator problems,

, where  is the pitch and

is the blade speed. The number of time steps in a period can

be determined by dividing the time period by the time step size. When the solution field does not

change from one period to the next (for example, if the change is less than %), a time-periodic

solution has been reached.

To determine how the solution changes from one period to the next, you must compare the solution

at some point in the flow field over two periods. For example, if the time period is  seconds, you

can compare the solution at a given point after  seconds with the solution after  seconds to see

if a time-periodic solution has been reached. If not, you can continue the calculation for another

period and compare the solutions after  and  seconds, and so on until you see little or no change

from one period to the next. You can also track global quantities, such as lift and drag coefficients

and mass flow, in the same manner. Figure . : Lift Coefficient Plot for a Time-Periodic Solution (p. )

shows a lift coefficient plot for a time-periodic solution.

Figure . : Lift Coefficient Plot for a Time-Periodic Solution

The final time-periodic solution is independent of the time steps taken during the initial stages of

the solution procedure. You can therefore define “large” time steps in the initial stages of the calcu-

lation, since you are not interested in a time-accurate solution for the startup phase of the flow.

Starting out with large time steps will allow the solution to become time-periodic more quickly. As

the solution becomes time-periodic, however, you should reduce the time step in order to achieve

a time-accurate result.

Important

If you are solving with second-order time accuracy, the temporal accuracy of the solution

will be affected if you change the time step during the calculation. You may start out with

larger time steps, but you should not change the time step by more than % during the

solution process. You should not change the time step at all during the last several periods

to ensure that the solution has approached a time-periodic state.

Postprocessing for sliding mesh problems is the same as for other transient problems. You will read

in the case and data file for the time of interest and display and report results as usual. For spatially-

periodic problems, you may want to use periodic repeats (set in the Views Dialog Box (p. ), as de-

scribed in Modifying the View (p. )) to display the geometry. Figure . : Contours of Static Pressure

for the Rotor-Stator Example (p. ) shows the flow field for the rotor-stator example in Figure . : Initial

Position of the Meshes (p. )) at one instant in time, using  periodic repeat.

Figure . : Contours of Static Pressure for the Rotor-Stator Example

When displaying velocity vectors, note that absolute velocities (that is, velocities in the inertial, or

laboratory, reference frame) are displayed by default. You may also choose to display relative velocities

by selecting Relative Velocity in the Vectors of drop-down list in the Vectors Dialog Box (p. ). In

this case, velocities relative to the translational/rotational velocity of the “reference zone” (specified

in the Reference Values Task Page (p. )) will be displayed. (The velocity of the reference zone is the

velocity defined in the Fluid Dialog Box (p. ) for that zone.)

Note that you cannot create zone surfaces for the intersection boundaries (that is, the interior/period-

ic/external zones created from the intersection of the interface zones). You may instead create zone

surfaces for the interface zones. Data displayed on these surfaces will be “one-sided”. That is, nodes

on the interface zones will “see” only the cells on one side of the mesh interface, and slight discontinu-

ities may appear when you plot contour lines across the interface. Note also that, for non-planar interface

shapes in 3D, you may see small gaps in your plots of filled contours. These discontinuities and gaps

are only graphical in nature. The solution does not have these discontinuities or gaps. To eliminate

these discontinuities for postprocessing purposes only, you can use the define/mesh-inter-

faces/enforce-continuity-after-bc? text command, which will ensure that continuity will

take precedence over the boundary condition.

Sliding mesh results can be analyzed by employing the time averaging (or RMSE averaging) option

(Data Sampling for Time Statistics) in the Run Calculation task page. This will compute time averages

for velocity, pressure, temperature, and turbulence. You must plan ahead since you have to engage

the time averaging after the solution has become time-periodic and run for at least one period of the

oscillating flow field.

The steps for setting up a dynamic mesh problem are listed below. (Note that this procedure includes

only those steps necessary for the dynamic mesh model itself; you must set up other models, cell zone

conditions, boundary conditions, and so on, as usual.)

. Enable the appropriate option for modeling transient or steady flow in the General Task Page (p. ).

Setup →

General

If your problem involves a steady flow, see Steady-State Dynamic Mesh Applications (p. ) for im-

portant considerations.

. Set cell zone conditions and boundary conditions as required in the Cell Zone Conditions Task Page (p. )

and Boundary Conditions Task Page (p. ).

Setup →

Setup →

See Cell Zone and Boundary Conditions (p. ) for information about inputting conditions. The

correct wall velocity is set up automatically when a dynamic zone is created for a wall zone and the

motion attributes are specified, so you will not specify wall motion in the Wall dialog box. If you

create a moving dynamic cell zone, then all wall boundaries adjacent to that cell zone will, by default,

impose the correct (moving) boundary conditions, and it is not necessary to declare these wall zones

as dynamic zones. Note that if a wall boundary mesh is moving because it belongs to an adjacent

moving dynamic cell zone, but the physical boundary conditions are such that the wall is actually

not moving, then you will have to declare this boundary as a dynamic zone and specify that the

mesh motion is not included in the boundary conditions (see Specifying the Motion of Dynamic

Zones (p. )).

. Enable the dynamic mesh model, and specify related parameters in the Dynamic Mesh Task Page (p. ).

Setup →

Dynamic Mesh →

Dynamic Mesh

See Setting Dynamic Mesh Modeling Parameters (p. ) for details.

. Create the dynamic zones for your model, using the Dynamic Mesh Zones Dialog Box (p. ).

Setup →

Dynamic Mesh → Create/Edit...

See Specifying the Motion of Dynamic Zones (p. ) for details.

. You can display the motion of the moving zones with prescribed motion to verify the simulation setup.

Setup →

Dynamic Mesh → Display Zone Motion...

See Previewing the Dynamic Mesh (p. ) for details.

. If it is a transient simulation, define the events that will occur during the calculation.

Setup →

Dynamic Mesh → Events...

See Defining Dynamic Mesh Events (p. ) for details.

. Save the case and data.

. Preview your dynamic mesh setup (when the motion is a prescribed motion). See Steady-State Dynamic

Mesh Applications (p. ) for previewing your steady-state dynamic mesh motion and refer to Previewing

the Dynamic Mesh (p. ) for details.

Setup →

Dynamic Mesh → Preview Mesh Motion...

. Specify the pressure-velocity coupling scheme. For transient flow calculations, the PISO algorithm is recom-

mended, as it is the most efficient for such cases (see PISO (p. ) for details).

. Use the automatic saving feature to specify the file name and frequency with which case and data files

should be saved during the solution process.

Solution → Calculation Activities → Autosave (Every) → Edit...

See Automatic Saving of Case and Data Files (p. ) for details about the use of this feature. This

provides a convenient way for you to save results at successive time steps for later postprocessing.

Important

in the proper position. You should also save your initial case file so that you can easily

return to the mesh’s original position to restart the solution if desired.

Using Dynamic Meshes

. (optional) If you want to create a graphical animation of the mesh over time during the solution procedure,

you can use the Calculation Activities Task Page (p. ) to set up the graphical displays that you want to

use in the animation. See Animating the Solution (p. ) for details.

... Setting Dynamic Mesh Modeling Parameters

... Dynamic Mesh Update Methods

... Feature Detection

... In-Cylinder Settings

... Six DOF Solver Settings

... Implicit Update Settings

... Contact Detection Settings

... Defining Dynamic Mesh Events

... Specifying the Motion of Dynamic Zones

... Previewing the Dynamic Mesh

... Steady-State Dynamic Mesh Applications

To enable the dynamic mesh model, enable Dynamic Mesh in the Dynamic Mesh Task Page (p. )

(Figure . : The Dynamic Mesh Task Page (p. )).

Setup →

Then, enable the appropriate options in the Options group box. If you are modeling in-cylinder motion,

Setup →

enable the In-Cylinder option. If you are going to use the six degrees of freedom solver, then enable

the Six DOF option. If you want to have the dynamic mesh updated during a time step (as opposed

to just at the beginning of a time step), then enable the Implicit Update option. More information

about these options and the related settings can be found in In-Cylinder Settings (p. ), Six DOF

Solver Settings (p. ), and Implicit Update Settings (p. ), respectively.

Next, you must select the appropriate mesh update methods in the Mesh Methods group box, and

set the associated parameters, if relevant. See Dynamic Mesh Update Methods (p. ) for details.

Figure . : The Dynamic Mesh Task Page

Three groups of mesh motion methods are available in ANSYS Fluent to update the volume mesh in

the deforming regions subject to the motion defined at the boundaries:

Smoothing Methods (p. )

Dynamic Layering (p. )

Remeshing Methods (p. )

Note that you can use ANSYS Fluent’s dynamic mesh models in conjunction with adaption, with the

exception of dynamic layering (in almost all cases) and any remeshing method other than CutCell zone

remeshing. For more information on the available adaption methods, see Hanging Node Adaption and

Polyhedral Unstructured Mesh Adaption in the Theory Guide.

Details on how to set up the various dynamic mesh update methods are provided in the sections that

follow.

.... Smoothing Methods

follow.

When smoothing is used to adjust the mesh of a zone with a moving and/or deforming boundary,

the interior nodes of the mesh move, but the number of nodes and their connectivity does not change.

In this way, the interior nodes “absorb” the movement of the boundary. To enable smoothing, perform

the following steps:

. Enable the Smoothing option in the Mesh Methods group box of the Dynamic Mesh Task Page (p. ).

. Click the Settings... button to open the Mesh Method Settings dialog box.

Figure . : The Smoothing Tab of the Mesh Method Settings Dialog Box

. If you want diffusion-based smoothing, select Diffusion from the Method list. Then click the

Advanced... button and define the settings in the Mesh Smoothing Parameters dialog box; for

details, see Diffusion-Based Smoothing (p. ).

Figure . : The Mesh Smoothing Parameters Dialog Box

. If you want spring-based smoothing, select Spring/Laplace/Boundary Layer from the Method

list. Then click the Advanced... button and define the settings in the Mesh Smoothing Parameters

dialog box; for details, see Spring-Based Smoothing (p. ).

. If you want smoothing using the linearly elastic solid method, select Linearly Elastic Solid from

the Method list. Then click the Advanced... button and define the settings in the Mesh

Smoothing Parameters dialog box; for details, see Linearly Elastic Solid Based Smoothing Meth-

od (p. ).

. If you selected Diffusion or Linearly Elastic Solid smoothing and the simulation involves periodic

od (p. ).

or quasi-periodic motion, you can specify that the smoothing uses a reference position. This option

may improve the mesh quality consistency from cycle to cycle—see Smoothing from a Reference

Position (p. ) for details.

. If you plan to apply the .5D remeshing method (as described in .5D Surface Remeshing Method (p. )),

perform the following steps to set up Laplacian smoothing (as described in Laplacian Smoothing Meth-

od (p. )).

a.

Select Spring/Laplace/Boundary Layer from the Method list

b. Click the Advanced... button and define only the Laplace Node Relaxation and the Maximum

Number of Iterations in the Mesh Smoothing Parameters group box (the other settings are

not relevant).

. If you plan to apply the boundary layer smoothing method (as described in Boundary Layer Smoothing

Method (p. )), select Spring/Laplace/Boundary Layer from the Method list.

..... Diffusion-Based Smoothing

For diffusion-based smoothing, the mesh motion is governed by the diffusion equation

(.)

where  is the mesh displacement velocity. The boundary conditions for Equation . (p. ) are

obtained from the user-prescribed or computed (six DOF) boundary motion. On deforming bound-

aries, the boundary conditions are such that the mesh motion is tangent to the boundary (that is,

the normal velocity component vanishes). The Laplace equation Equation . (p. ) then describes

how the prescribed boundary motion diffuses into the interior of the deforming mesh.

The diffusion coefficient  in Equation . (p. ) can be used to control how the boundary motion

affects the interior mesh motion. A constant coefficient means that the boundary motion diffuses

uniformly throughout the mesh. With a nonuniform diffusion coefficient, mesh nodes in regions

with high diffusivity tend to move together (that is, with less relative motion).

In Fluent, two different formulations for the diffusion coefficient  are available for selection from

the Diffusion Function drop-down list in the Mesh Smoothing Parameters Dialog Box (p. ). The

first formulation allows you to have the diffusion coefficient be a function of the Boundary Distance,

and is of the form

(.)

where  is a normalized boundary distance. The second formulation allows you to have the diffusion

coefficient be a function of the Cell Volume, and is of the form

(.)

where

is the normalized cell volume. In both Equation . (p. ) and Equation . (p. ),

is a user input parameter. See Diffusivity Based on Boundary Distance (p. ) and Diffusivity Based

on Cell Volume (p. ) for information about defining the diffusion coefficient.

ANSYS Fluent uses different numerical methods to solve the vector Equation . (p. ), depending

on the element types present in the mesh. In the absence of polyhedral elements or elements with

hanging nodes (that is, meshes that have undergone hanging node adaption and some hexcore or

CutCell meshes) the equation is solved using a finite element discretization and the displacement

velocity,

, is obtained directly at each mesh node. If the mesh contains polyhedral elements or

hanging nodes, the equation is discretized using ANSYS Fluent’s standard finite volume method and

the cell-centered solution for the displacement velocity,

, is interpolated onto the nodes using in-

verse-distance-weighted averaging. The node positions are then updated according to:

(.)

The finite element discretization is generally superior, as the solution is obtained directly at the

nodes and no interpolation step is necessary. The finite volume method can be enforced for meshes

of all element types by executing the TUI command:

/define/dynamic-mesh/controls/smoothing-parameters/diffusion-fvm? yes

With finite element discretization, you can specify the solution method used by the linear solver for

the diffusion-based smoothing calculations. By default, the CG (conjugate gradient) method is selected

from the AMG Stabilization drop-down list. This method should be faster in this context than the

other available methods, as it takes advantage of the symmetry of the matrix used in the linear

systems of equations of finite-element-based mesh smoothing. If divergence is detected with CG,

then the generalized minimal residual (GMRES) method will be used for an iteration as a fallback,

and you will be informed in the console that a finite-element-based mesh smoothing coupled

equation is being stabilized to enhance linear solver robustness. In rare cases, the CG method may

result in the generation of negative volume cells; you may be able to avoid this by increasing the

Maximum Number of Iterations from the default of  to a value in the range of –.

If the CG method continues to generate negative volume cells with a higher number of iterations

or if you repeatedly see console messages that say the GMRES fallback is being used, it is recommen-

ded that you select GMRES from the AMG Stabilization drop-down list. Note that the GMRES

method is more robust than the CG method, especially for high-aspect-ratio meshes; but it is also

more demanding in terms of memory usage and solver time.

Note that this drop-down list also allows you to select the BCGSTAB (bi-conjugate gradient stabilized)

method; like the CG method, BCGSTAB falls back to the GMRES method for an iteration when diver-

gence is detected.

Computationally, solving a PDE for mesh smoothing is generally more costly than spring-based

smoothing. But it tends to produce better quality meshes than spring-based smoothing and often

allows larger boundary deformations before breaking down. Figure . : The Initial Mesh (p. )

and Figure . : Valid Mesh After  Degree Rotation Using Diffusion-Based Smoothing (p. ) show

a mesh before and after rotating the boundary by  degrees, using diffusion-based smoothing.

With spring-based smoothing, the same mesh shows degenerated cells after a rotation of  degrees

(Figure . : Degenerated Mesh After  Degree Rotation Using Spring-Based Smoothing (p. )).

Figure . : The Initial Mesh

Figure . : Valid Mesh After  Degree Rotation Using Diffusion-Based Smoothing

Figure . : Degenerated Mesh After  Degree Rotation Using Spring-Based Smoothing

It should be noted that with diffusion-based smoothing the interior mesh motion is governed by

the solution to Equation . (p. ) and the prescribed boundary motion, and not by mesh irregu-

larities. Poor quality elements or mesh defects are not smoothed out by this method, but rather

move together with the pre-computed (at the begin of each mesh update) displacement velocity

.

It is also worth noting that the nature of the diffusion equation is such that the resulting solution

(that is, the displacement velocity ) depends on the dimensionality of the problem and the type

of boundary motion prescribed. To illustrate the impact of the type of boundary motion, consider

the goal of boundary-distance-based diffusion (Equation . (p. )): to control which parts of the

mesh absorb the boundary motion, so that you can preserve the mesh in the vicinity of the moving

boundary (at the expense of the interior of the mesh). For more translational (piston-type) boundary

motions, you can preserve a reasonably “thick” region of the mesh adjacent to the boundary (that

is, multiple layers of cells); for rotational boundary motions, the rate of decay for the solution as you

move away from the boundary is such that it can be difficult to preserve even a “thin” region. For

this reason, mesh smoothing can handle translational boundary motions generally much better than

rotational motions.

Although it should in most cases not be necessary, the accuracy of the solution to the diffusion

equation governing the mesh motion can be controlled by defining the Maximum Number of Iter-

ations and the Relative Convergence Tolerance.

You can enable printing of smoothing residuals in the console by entering  for the Verbosity.

For simulations with periodic or quasi-periodic motion, you can improve the mesh quality consistency

by specifying that the diffusion-based smoothing uses a reference position, as described in

Smoothing from a Reference Position (p. ).

...... Diffusivity Based on Boundary Distance

Using boundary-distance-based diffusion (Equation . (p. )) allows you to control how the

boundary motion diffuses into the interior of the domain as a function of boundary distance. De-

creasing the diffusivity away from the moving boundary causes those regions to absorb more of the

mesh motion, and better preserves the mesh quality near the moving boundary. This is particularly

helpful for a moving boundary that has pronounced geometrical features (such as sharp corners)

along with a prescribed motion that is predominantly rotational.

You can manipulate the diffusion coefficient  (in Equation . (p. )) primarily by adjusting the

Diffusion Parameter in the Mesh Smoothing Parameters Dialog Box (p. ) ( ). A range of  to

has been shown to be of practical use. A value of  (the default value) specifies that

and yields

a uniform diffusion of the boundary motion throughout the mesh. Higher values of  preserve larger

regions of the mesh near the moving boundary, and cause the regions away from the moving

boundary to absorb more of the motion.

The following two figures illustrate the effect of the Diffusion Parameter

on the resulting mesh

for a translational (piston-type) boundary motion, when the diffusivity is based on the boundary

distance. In this example, an initially uniformly meshed square domain is deformed by moving the

left boundary to the right.

Figure . : Effect of Diffusion Parameter of  on Interior Node Motion

For rotational boundary motions, a value of . for the Diffusion Parameter

is recommended as

a good starting point.

Two different methods are available for the evaluation of the boundary distance  if boundary-dis-

tance-based diffusion is used. By default, Fluent uses the “standard” boundary distance in Equa-

tion . (p. ), which is the normalized distance to the nearest wall boundary; note that none of

the other boundary types (for example, inlets, outlets, symmetry, and periodic boundaries) are con-

sidered. This method is the same as that which is used to evaluate the boundary distance for turbu-

lence models. An example of this method is shown in Figure . : Effect of Diffusion Parameter of

on Interior Node Motion (p. ), where only the left and right boundaries are walls. You have the

option of enabling the Generalized Boundary Distance Method option instead, so that  is the

normalized distance to the nearest boundary that is not declared as deforming, regardless of type.

Both methods use the largest distance found in all deforming cell zones to normalize the value.

If the generalized boundary distance is used, an additional scalar equation for the boundary distance

will be solved as part of the solution of Equation . (p. ).

...... Diffusivity Based on Cell Volume

Using cell-volume-based diffusion (Equation . (p. )) allows you to control how the boundary

motion diffuses into the interior of the domain as a function of cell size. Decreasing the diffusivity

in larger cells causes those cells to absorb more of mesh motion and therefore better preserves the

cell quality of smaller cells.

You can manipulate the diffusion coefficient  (in Equation . (p. )) by adjusting the Diffusion

Parameter in the Mesh Smoothing Parameters Dialog Box (p. ) ( ). A value of  (the default

value) specifies that

and yields a uniform diffusion of the boundary motion throughout the

mesh. Higher values of  result in larger cells absorbing more of the motion than smaller cells.

Note that the cell volume used in Equation . (p. ) is the local cell volume, normalized by the

average cell volume of all deforming cell zones.

...... Applicability of the Diffusion-Based Smoothing Method

Diffusion-based mesh smoothing is an alternative method to spring-based smoothing. It is available

for all element types, and you can use it to update any cell zone whose boundaries are moving or

deforming.

Diffusion-based smoothing is computationally more expensive than spring-based smoothing, but

likely results in better mesh quality (especially for non-tetrahedral / non-triangular cell zones, and

for polyhedral cells in particular) and generally allows for larger boundary deformations before

breaking down.

Similar to spring-based smoothing, diffusion-based mesh smoothing can handle translational

boundary deformations much better than rotational motions.

Diffusion-based smoothing is not compatible with the boundary layer smoothing method or the

face region remeshing method. For more information about these methods, see Boundary Layer

Smoothing Method (p. ) and Face Region Remeshing Method (p. ).

..... Spring-Based Smoothing

For spring-based smoothing, the edges between any two mesh nodes are idealized as a network of

interconnected springs. The initial spacings of the edges before any boundary motion constitute

the equilibrium state of the mesh. A displacement at a given boundary node will generate a force

proportional to the displacement along all the springs connected to the node. Using Hook’s Law,

the force on a mesh node can be written as

(.)

where

and

are the displacements of node  and its neighbor ,

is the number of neigh-

boring nodes connected to node , and

is the spring constant (or stiffness) between node  and

its neighbor . The spring constant for the edge connecting nodes  and  is defined as

(.)

where

is the value you enter for Spring Constant Factor in the Mesh Smoothing Parameters

At equilibrium, the net force on a node due to all the springs connected to the node must be zero.

This condition results in an iterative equation such that

(.)

where

is the iteration number.

Since displacements are known at the boundaries (after boundary node positions have been updated),

Equation . (p. ) is solved using a Jacobi sweep on all interior nodes. At convergence, the posi-

tions are updated such that

(.)

where

and  are used to denote the positions at the next time step and the current time step,

(.)

where

respectively. The spring-based smoothing is shown in Figure . : Spring-Based Smoothing on In-

terior Nodes: Start (p. ) and Figure . : Spring-Based Smoothing on Interior Nodes: End (p. )

for a cylindrical cell zone where one end of the cylinder is moving.

Figure . : Spring-Based Smoothing on Interior Nodes: Start

Figure . : Spring-Based Smoothing on Interior Nodes: End

You can control the spring stiffness by adjusting the value of the Spring Constant Factor between

and . A value of  indicates that there is no damping on the springs, and boundary node displace-

ments have more influence on the motion of the interior nodes. A value of  imposes the default

level of damping on the interior node displacements as determined by solving Equation . (p. ).

The effect of the Spring Constant Factor is illustrated in Figure . : Interior Nodes Extend Beyond

Boundary (Spring Constant Factor = ) (p. ) and Figure . : Interior Nodes Remain Within

Boundary (Spring Constant Factor = ) (p. ), which show the trailing edge of a NACA- airfoil

after a counter-clockwise rotation of .° and the mesh is smoothed using the spring-based

smoother but limited to  iterations. Degenerate cells (Figure . : Interior Nodes Extend Beyond

Boundary (Spring Constant Factor = ) (p. )) are created with the default value of  for the Spring

Constant Factor, as the interior nodes extend beyond the moving boundary. However, the original

mesh distribution (Figure . : Interior Nodes Remain Within Boundary (Spring Constant Factor =

) (p. )) is recovered if the Spring Constant Factor is set to  (that is, no damping on the displace-

ment of interior nodes near the airfoil surface).

Figure . : Interior Nodes Extend Beyond Boundary (Spring Constant Factor = )

Figure . : Interior Nodes Remain Within Boundary (Spring Constant Factor = )

You can control the solution of Equation . (p. ) using the values of Convergence Tolerance

and Maximum Number of Iterations. ANSYS Fluent solves Equation . (p. ) iteratively during

each time step until one of the following criteria is met:

The specified number of iterations has been performed.

The solution is converged for that time step:

(.)

where

is the interior and deforming nodes RMS displacement at the first iteration.

...... Applicability of the Spring-Based Smoothing Method

You can use the spring-based smoothing method to update any cell or face zone whose boundary

is moving or deforming.

For non-tetrahedral cell zones (non-triangular in 2D), the spring-based method can be used when

the following conditions are met:

The boundary of the cell zone moves predominantly in one direction (that is, no excessive anisotropic

stretching or compression of the cell zone).

The motion is predominantly normal to the boundary zone.

If these conditions are not met, the resulting cells may have high skewness values, since not all

possible combinations of node pairs in non-tetrahedral cells (or non-triangular in 2D) are idealized

as springs. Polyhedral cells are particularly likely to become highly skewed with spring-based

smoothing (regardless of whether the previous conditions are met), and so the diffusion-based

smoothing method is generally recommended for polyhedra (see Diffusion-Based Smoothing (p. )).

By default, spring-based smoothing is enabled for all cell zones. This is reflected in the Mesh

Smoothing Parameters Dialog Box (p. ), where All is selected from the Elements list. If you want

to disable spring-based smoothing for cell zones that are not entirely composed of either tetrahedral

or triangular cells, you can do that by selecting Tet in Tet Zones in 3D (or Tri in Tri Zones in 2D).

If you have mixed element zones and you do not want spring-based smoothing on all element types,

you can enable spring-based smoothing on only the tetrahedral or triangular cells by selecting Tet

in Mixed Zones in 3D (or Tri in Mixed Zones in 2D). Selection of smoothing elements in the Mesh

Smoothing Parameters Dialog Box (p. ) applies by default to all cell zones that undergo spring-

based smoothing. In order to have more precise control, it is possible to overwrite this global selection

on individual dynamic cell zones (see Deforming Motion (p. )). This gives, for example, the flexib-

ility to suppress smoothing in zones where dynamic layering (see Dynamic Layering (p. )) is used

and allows at the same time smoothing of non-simplex (that is not tetrahedral or triangular) elements

in other zones.

..... Linearly Elastic Solid Based Smoothing Method

With mesh smoothing based on the linearly elastic solid model, the mesh motion is governed by

the following set of equations.

(.)

where  is the stress tensor,

is the strain tensor, and  is the mesh displacement. For the solution

of Equation . (p. ) only the ratio between the shear modulus,

, and Lamé’s first parameter,

, matters. This ratio is parameterized through Poisson’s ratio ( ):

(.)

You define this property through the Poisson's Ratio field in the Mesh Smoothing Parameters Dialog

Box (p. ). Note that the linearly elastic solid mesh smoothing model supports constant material

properties only. The permissible range for Poisson's Ratio is between -. and ..

The boundary conditions for Equation . (p. ) are obtained from the user-prescribed or computed

(in the case of six DOF motion) boundary deformations. These imposed deformations are transferred

into the interior of the deforming mesh as if the mesh was a linearly elastic solid with the given

material properties. On deforming boundaries you can either specify a geometry along which the

mesh can slide, or leave the geometry unspecified. If a geometry is specified for the deforming

boundary, then the boundary conditions are such that the deformation normal to the boundary

vanishes and the stress tangential to the boundary is zero. If the geometry of the deforming

boundary is unspecified, then the deforming boundary can also deform in the normal direction and

the boundary conditions are such that the traction is zero in all directions. See Deforming Mo-

tion (p. ) for details of how to specify geometry on deforming zones.

The linear system in Equation . (p. ) is solved using a finite element discretization and the

mesh displacements for the interior and deforming boundary nodes are obtained directly at the

nodes. The accuracy to which the linear system is solved can be controlled by the Maximum Number

of Iterations and the Relative Convergence Tolerance.

You can specify the solution method used by the linear solver for the linearly elastic solid mesh

smoothing calculations. By default, the CG (conjugate gradient) method is selected from the AMG

Stabilization drop-down list. This method should be faster in this context than the other available

methods, as it takes advantage of the symmetry of the matrix used in the linear systems of equations

of finite-element-based mesh smoothing. If divergence is detected with CG, then the generalized

minimal residual (GMRES) method will be used for an iteration as a fallback, and you will be informed

in the console that a finite-element-based mesh smoothing coupled equation is being stabilized to

enhance linear solver robustness. In rare cases, the CG method may result in the generation of

negative volume cells; you may be able to avoid this by increasing the Maximum Number of Itera-

tions from the default of  to a value in the range of –.

If the CG method continues to generate negative volume cells with a higher number of inner iterations

by specifying that the linearly elastic solid mesh smoothing uses a reference position, as described

in Smoothing from a Reference Position (p. ).

...... Applicability of the Linearly Elastic Solid Based Smoothing Method

Mesh smoothing based on the linearly elastic solid model is an alternative method to diffusion-based

and spring-based smoothing. Most of the properties and limitations discussed for diffusion-based

smoothing (Applicability of the Diffusion-Based Smoothing Method (p. )) also apply to the linearly

elastic solid model, particularly the mesh quality degradation for rotational motions. The linearly

elastic solid model is computationally more expensive than diffusion-based smoothing, but for some

meshes and mesh motions preserves the mesh quality better.

The current implementation with constant material properties can be a limitation compared with

diffusion-based smoothing with non-uniform diffusivity. In cases with rotational boundary motion

and sharp corners it may be advantageous to use diffusion-based smoothing with boundary-distance-

dependent diffusivity.

The option to leave the geometry of deforming face zones unspecified is only available with the

linearly elastic solid smoothing method.

The linearly elastic solid smoothing method supports triangular and quadrilateral elements in 2D

and tetrahedral, hexahedral, wedge, and pyramid cells in 3D. It cannot be applied if the deforming

cell zone contains polyhedral cells or hanging nodes. In such cases diffusion-based smoothing is

recommended.

Linearly elastic solid smoothing is not compatible with the boundary layer smoothing method or

the face region remeshing method. For more information about these methods, see Boundary Layer

..... Smoothing from a Reference Position

When the mesh smoothing is based on diffusion or the linearly elastic solid model, you have the

option of specifying that the smoothing uses a reference position. This can be helpful when perform-

ing many cycles of periodic or quasi-periodic motion for stationary or moving meshes; for example,

turbomachinery rotors with blade flutter. When you ensure that the smoothing is always done from

the same reference position, the mesh quality may remain more consistent from cycle to cycle.

To use this feature, enable the Smoothing From Reference Position option in the Mesh Smoothing

Parameters Dialog Box (p. ). Note this option is enabled by default during the calculation if the

case includes a cell zone that has Frame Motion or Mesh Motion enabled with a nonzero rotational

velocity and that is also defined as a deforming dynamic mesh zone. This option is not available if

the Layering and/or Remeshing options are enabled in the Dynamic Mesh task page, or if Dynamic

Adaption is enabled in the Adaption Controls dialog box.

The reference position is saved the first time you perform smoothing after enabling this option. It

is recommended that you save your case / data files using the Hierarchical Data Format (HDF); oth-

erwise, the reference position is not saved, and so restarting from a .cas file will imply that a dif-

ferent reference position is used after restart. This still provides the benefit of consistent quality, but

the resulting meshes might be slightly different from a continuous run. The impact of such slight

mesh changes on the solution results will be small, except for cases with a high degree of mesh

dependence; if you cannot use an HDF file for such exceptional cases (for example, when running

Fluent under ANSYS Workbench), it is recommended that you evaluate the original mesh to ensure

that it is suitable for the problem.

..... Laplacian Smoothing Method

Laplacian smoothing is the most commonly used and the simplest mesh smoothing method. This

method adjusts the location of each mesh vertex to the geometric center of its neighboring vertices.

This method is computationally inexpensive but it does not guarantee an improvement on mesh

quality, since repositioning a vertex by Laplacian smoothing can result in poor quality elements. To

overcome this problem, ANSYS Fluent only relocates the vertex to the geometric center of its

neighboring vertices if and only if there is an improvement in the mesh quality (that is, the skewness

has been improved).

This improved Laplacian smoothing can be enabled on deforming boundaries only (that is, the zone

with triangular elements in 3D and zones with linear elements in 2D). The computation of the node

positions works as follows:

(.)

where

is the averaged node position of node  at iteration

,

is the node position of

neighbor node of

at iteration

, and

is the number nodes neighboring node . The new node

position

is then computed as follows:

(.)

where  is the Laplace node relaxation factor.

This update only happens if the maximum skewness of all faces adjacent to

is improved in

comparison to

.

For details on applying Laplacian smoothing to either a cell zone (with .5D remeshing) or a face

zone, see Smoothing Methods (p. ) or Deforming Motion (p. ), respectively.

..... Boundary Layer Smoothing Method

The boundary layer smoothing method is used to deform the boundary layer mesh during a moving-

deforming mesh simulation. For cases that apply mesh motion (either Rigid Body or User-Defined)

to a face zone with adjacent boundary layers, the boundary layers can be made to deform accordingly

by enabling Deform Adjacent Boundary Layer with Zone for the face zone in the Dynamic Mesh

Zones Dialog Box (p. ). With boundary layer smoothing enabled, the nodal coordinates of each

cell in the boundary layer zone are updated with the same displacement vector as the corresponding

nodes on the underlying face zone. The boundary layer smoothing method can be applied to

boundary layer zones of all mesh types (that is, wedges and hexahedra in 3D, quadrilaterals in 2D).

Consider the example below, where a UDF of the form DEFINE_GRID_MOTION provides the

moving-deforming mesh model with the locations of the nodes located on the compliant strip on

an idealized airfoil. The node motion varies sinusoidally in time and space (compare Figure . : The

Undeformed Mesh (p. ) with Figure . : The Deformed Mesh (p. )).

Figure . : The Undeformed Mesh

Figure . : The Deformed Mesh

As a result of the boundary layer smoothing, the cells adjacent to the deforming wall are also de-

formed in order to preserve the quality of boundary layer zone. If you compare Figure . : Zooming

into the Undeformed Compliant Strip (p. ) with Figure . : Zooming into the Deformed Compliant

Strip with Boundary Layer Smoothing Applied (p. ), you can see how the boundary layer cells

have been deformed according to the motion of the nodes on the compliant strip.

Figure . : Zooming into the Undeformed Compliant Strip

Figure . : Zooming into the Deformed Compliant Strip with Boundary Layer Smoothing

Applied

Applied

Typically, the boundary layer smoothing method preserves the height of the boundary layer cells

adjacent to the deformed face zone. However, note that this approach is primarily intended for

translational motion. If the faces undergo substantial rotation, the boundary layer cells may become

skewed. See Smoothing Methods (p. ) and Specifying Boundary Layer Deformation Smooth-

ing (p. ) for details about enabling smoothing and defining a moving and deforming boundary

layer, respectively. Note that boundary layer smoothing is compatible with spring-based smoothing

only. It cannot be used with diffusion-based smoothing or linearly elastic solid smoothing. Also note

that the boundary layer smoothing method will work whether or not you have segregated the

boundary layer elements into a separate cell zone.

.... Dynamic Layering

In prismatic (hexahedral and/or wedge) mesh zones, you can use dynamic layering to add or remove

layers of cells adjacent to a moving boundary, based on the height of the layer adjacent to the

moving surface. The dynamic mesh model in ANSYS Fluent allows you to specify an ideal layer height

on each moving boundary. The layer of cells adjacent to the moving boundary (layer  in Fig-

ure . : Dynamic Layering (p. )) is split or merged with the layer of cells next to it (layer  in

Figure . : Dynamic Layering (p. )) based on the height ( ) of the cells in layer .

Figure . : Dynamic Layering

If the cells in layer  are expanding, the cell heights are allowed to increase until

(.)

where

(.)

where

is the minimum cell height of cell layer ,

is the ideal cell height, and

is the layer

split factor. Note that ANSYS Fluent allows you to define

as either a constant value or a value

that varies as a function of time or crank angle. When the condition in Equation . (p. ) is met,

the cells are split based on the specified layering option. This option can be height based or ratio

based.

With the height-based option, the cells are split to create a layer of cells with constant height

and a layer of cells of height

. With the ratio-based option the cells are split such that, locally,

the ratio of the new cell heights to old cell heights is exactly

everywhere. Figure . : Results of

Splitting Layer with the Height-Based Option (p. ) and Figure . : Results of Splitting Layer with

the Ratio-Based Option (p. ) show the result of splitting a layer of cells above a valve geometry

using the height-based and ratio-based option.

Figure . : Results of Splitting Layer with the Height-Based Option

Figure . : Results of Splitting Layer with the Ratio-Based Option

If the cells in layer  are being compressed, they can be compressed until

(.)

where

is the layer collapse factor. When this condition is met, the compressed layer of cells is

merged into the layer of cells above the compressed layer in Figure . : Dynamic Layering (p. );

that is, the cells in layer  are merged with those in layer .

To enable dynamic layering, enable the Layering option under Mesh Methods in the Dynamic Mesh

Task Page (p. ) (Figure . : The Layering Tab in the Mesh Method Settings Dialog Box (p. )).

The layering control is specified in the Layering tab, which can be displayed by clicking Settings....

Figure . : The Layering Tab in the Mesh Method Settings Dialog Box

You can control how a cell layer is split by specifying either Height Based or Ratio Based under

Options. Note that for Height Based, the height of the cells in a particular new layer will be constant,

but you can choose to have this height vary from layer to layer as a function of time or crank angle

when you specify the Cell Height in the Dynamic Mesh Zones dialog box (see Specifying the Motion

of Dynamic Zones (p. ) for further details).

The Split Factor and Collapse Factor (

in Equation . (p. ) and

respectively) are the factors that determine when a layer of cells (hexahedra or wedges in 3D, or

quadrilaterals in 2D) that is next to a moving boundary is split or merged with the adjacent cell layer,

respectively.

..... Applicability of the Dynamic Layering Method

You can use the dynamic layering method to split or merge cells adjacent to any moving boundary

provided the following conditions are met:

All cells adjacent to the moving face zone are either wedges or hexahedra (quadrilaterals in 2D) even

though the cell zone may contain mixed cell shapes.

The cell layers must be completely bounded by one-sided face zones, except when sliding interfaces are

used (see Applicability of the Face Region Remeshing Method (p. )).

Note that you cannot use the dynamic layering method in conjunction with adaption in almost all cases.

For more information on the available adaption methods, see Hanging Node Adaption and Polyhedral

Unstructured Mesh Adaption in the Theory Guide.

If the moving boundary is an internal zone, cells on both sides (possibly with different ideal cell

layer heights) of the internal zone are considered for dynamic layering.

If you want to use dynamic layering on cells adjacent to a moving wall that do not span from

boundary to boundary, you must separate those cells that are involved in the dynamic layering and

use the sliding interfaces capability in ANSYS Fluent to transition from the deforming cells to the

adjacent non-deforming cells (see Figure . : Use of Sliding Interfaces to Transition Between Adjacent

Cell Zones and the Dynamic Layering Cell Zone (p. )). For a moving interior face, the zones must

be separated such that they are either expanding or collapsing on the same side. No one zone can

consist of both expanding and collapsing layers.

Figure . : Use of Sliding Interfaces to Transition Between Adjacent Cell Zones and the

Dynamic Layering Cell Zone

.... Remeshing Methods

When the boundary displacement is large compared to the local cell sizes, the cell quality can deteri-

orate or the cells can become degenerate if only mesh smoothing is used. This will invalidate the

mesh (for example, result in negative cell volumes) and consequently, will lead to convergence

problems when the solution is updated to the next time step.

To circumvent this problem, ANSYS Fluent agglomerates cells that violate the skewness or size criteria

and locally remeshes the agglomerated cells or faces. If the new cells or faces satisfy the skewness

criterion, the mesh is locally updated with the new cells (with the solution interpolated from the old

cells). Otherwise, the new cells are discarded and the old cells are retained.

ANSYS Fluent includes several remeshing methods that include local cell remeshing, zone remeshing,

local face remeshing (for 3D flows only), face region remeshing, CutCell zone remeshing (for 3D flows

only), and .5D surface remeshing (for 3D flows only). The remeshing methods are suitable for partic-

ular kinds of cell types:

The local cell remeshing method only affects triangular and tetrahedral cell types in the mesh (that is, in

mixed cell zones the non-triangular/tetrahedral cells are skipped).

The local face remeshing method is available in 3D only and can remesh tetrahedral cells and wedge cells

in boundary layer meshes.

The zone remeshing method replaces all cell types with triangular tetrahedral cells (in 2D and 3D domains,

respectively), and can remesh and produce wedge cells in 3D boundary layer meshes.

The face region remeshing method is applied to triangular cells in 2D, and tetrahedral cells in 3D. In 3D

domains, the face region remeshing method can also remesh and produce wedge cells in 3D boundary

layer meshes.

The CutCell zone remeshing method works for all cell types.

The .5D remeshing method only works on hexagonal meshes or wedge cells extruded from triangular

surface elements.

To enable remeshing methods, enable the Remeshing option under Mesh Methods in the Dynamic

Mesh Task Page (p. ) (Figure . : The Dynamic Mesh Task Page (p. )). Click the Settings...

button to open the Mesh Method Settings dialog box, where you can specify the remeshing method

and parameters in the Remeshing tab (Figure . : The Remeshing Tab in the Mesh Method Settings

You can view the vital statistics of your mesh by clicking the Mesh Scale Info... button at the bottom

of the Mesh Method Settings Dialog Box (p. ). This button opens the Mesh Scale Info Dialog

Box (p. ), where you can view the minimum and maximum length scale values, as well as the

maximum cell and face skewness values.

Figure . : The Remeshing Tab in the Mesh Method Settings Dialog Box

Figure . : The Remeshing Tab in the Mesh Method Settings Dialog Box Using the Sizing

Function Option

..... Local Remeshing Method

Using the local remeshing method (that is, local cell remeshing, with or without local face remeshing),

ANSYS Fluent marks cells based on cell skewness and minimum and maximum length scales as well

as an optional sizing function.

ANSYS Fluent evaluates each cell and marks it for remeshing if it meets one or more of the following

criteria:

It has a skewness that is greater than a specified maximum skewness.

It is smaller than a specified minimum length scale.

It is larger than a specified maximum length scale.

Its height does not meet the specified length scale (at moving face zones, for example, above a moving

piston).

If local remeshing is not able to reduce the maximum cell skewness sufficiently, then the cell zone

piston).

remeshing method is used to automatically remesh all of the cells in the cell zone, as well as the

faces of all adjacent deforming dynamic face zones (see Cell Zone Remeshing Method (p. ) for

details). The maximum allowable cell skewness is set to be . by default. The cell zone remeshing

method gives the mesher more flexibility to create a new mesh of better quality than the local cell

remeshing method. The automatic remeshing of cell zones can be disabled using the following text

command:

define → dynamic-mesh → controls → remeshing-parameter → zone-remeshing

...... Local Cell Remeshing Method

As previously mentioned, in local cell remeshing, ANSYS Fluent agglomerates cells based on skewness,

size, and height (adjacent moving face zones) prior to the movement of the boundary. The size cri-

teria are specified with Minimum Length Scale and Maximum Length Scale. Cells with length

scales below the minimum length scale and above the maximum length scale are marked for

remeshing. The value of Maximum Cell Skewness indicates the desired skewness of the mesh. By

default, the Maximum Cell Skewness is set to . for 3D simulations and . for 2D simulations.

Cells with skewness above the maximum skewness are marked for remeshing.

The marking of cells based on skewness is done at every time step when the local remeshing

method is enabled. However, marking based on size and height is performed between the specified

Size Remeshing Interval since the change in cell size distribution is typically small over one time

step.

step.

Note that you should edit the fields in the Parameters group box, as the initial values are unlikely

to produce your desired outcome. Clicking Default will define values that are based on your partic-

ular mesh and that should represent a reasonable starting point, and you can then adjust them as

needed. After you click the Default button, it will then change to be a Reset button, which can be

used to return to the prior values.

By default, ANSYS Fluent replaces the agglomerated cells only if the quality of the remeshed cells

has improved.

Note that you cannot use the local cell remeshing method in conjunction with adaption. For more

information on the available adaption methods, see Hanging Node Adaption and Polyhedral Unstruc-

tured Mesh Adaption in the Theory Guide.

...... Local Face Remeshing Method

The local face remeshing method only applies to 3D geometries. You can apply this method to the

boundaries of deforming or user-defined zone types, so that ANSYS Fluent will mark faces (and ad-

jacent cells) based on the face skewness, and then remesh them.

Local face remeshing also allows the remeshing of wedge cells in boundary layers at those bound-

aries. The detection of boundary layers (as well as the wedge element height distribution and

number of layers) is automatic and does not require your input.

To apply local face remeshing, perform the following steps:

. Enable the Local Face option in the Remeshing tab of the Mesh Method Settings Dialog Box (p. ),

and set the Maximum Face Skewness to an appropriate global value.

. For each deforming or user-defined boundary zone on which you want local face remeshing

applied, enable the Local option in the Meshing Options tab of the Dynamic Mesh Zones Dialog

Box (p. ). You can also revise the Maximum Skewness in this tab if you don't want to use the

global setting for a particular zone. Note that for deforming zones, the Remeshing option must

be enabled—which is the default condition—in order to access the Local option, and the

Global Settings option must be disabled to revise the Maximum Skewness. For further details

on the zone setup, see Deforming Motion (p. ) and/or User-Defined Motion (p. ).

....... Applicability of the Local Face Remeshing Method

When you enable local face remeshing for a boundary, the faces can be remeshed only if the following

conditions are met:

The faces are triangular.

The agglomerated faces do not span multiple zones or feature edges.

Note that you cannot use the local face remeshing method in conjunction with adaption. For more

...... Local Remeshing Based on Sizing Function

Instead of marking cells based on minimum and maximum length scales, ANSYS Fluent also marks

cells based on the size distribution generated by the sizing function if the Sizing Function option

is enabled.

Cells can be marked using sizing functions only with the following remeshing methods:

local cell remeshing

.5D surface remeshing (as described in .5D Surface Remeshing Method (p. ))

Figure . : Mesh at the End of a Dynamic Mesh Simulation With Sizing Functions (p. ) demon-

strates the advantages of using sizing functions for local remeshing.

Figure . : Mesh at the End of a Dynamic Mesh Simulation Without Sizing Functions

Figure . : Mesh at the End of a Dynamic Mesh Simulation With Sizing Functions

In determining the sizing function, ANSYS Fluent draws a bounding box around the zone that is

approximately twice the size of the zone, and locates the shortest feature length within each fluid

zone. ANSYS Fluent then subdivides the bounding box based on the shortest feature length and the

sizing function Resolution that you specify. This allows ANSYS Fluent to create a background mesh.

You control the resolution of the background mesh and a background mesh is created for each fluid

zone. The shortest feature length is determined by shrinking a second box around the object, and

then selecting the shortest edge on that box. The sizing function is evaluated at the vertex of each

individual background mesh.

Figure . : Sizing Function Determination at Background Mesh Vertex I

As seen in Figure . : Sizing Function Determination at Background Mesh Vertex I (p. ), the

local value of the sizing function

(.)

where

is the distance from vertex  on the background mesh to the centroid of boundary cell

and

is the mesh size (length) of boundary cell .

The sizing function is then smoothed using Laplacian smoothing. ANSYS Fluent then interpolates

the value of the sizing function by calculating the distance

from a given cell centroid  to the

background mesh vertices that surround the cell (see Figure . : Interpolating the Value of the

Sizing Function (p. )). The intermediate value of the sizing function

at the centroid is computed

from

(.)

Figure . : Interpolating the Value of the Sizing Function

Next, a single point

is located within the domain (see Figure . : Determining the Normalized

Distance (p. )) that has the largest distance

to the nearest boundary to it. The normalized

distance

for the given centroid  is given by

(.)

Figure . : Determining the Normalized Distance

Using the parameters  and  (the sizing function Variation and the sizing function Rate, respect-

ively), you can write the final value

of the sizing function at point  as

(.)

where

is the intermediate value of the sizing function at the cell centroid.

Note that  is the sizing function variation. Positive values mean that the cell size increases as you

move away from the boundary. Since the maximum value of

is one, the maximum cell size becomes

(.)

therefore,

is really a measure of the maximum cell size.

The factor  is computed from

(.)

(.)

You can use sizing function Variation (or ) to control how large or small an interior cell can be

with respect to its closest boundary cell.

ranges from

to

, an  value of . indicates that

the interior cell size can be, at most, . the size of the closest boundary cell. Conversely, an  value

of

indicates that the cell size interior of the boundary can be half of that at the closest

of

boundary cell. A value of  indicates a constant size distribution away from the boundary.

You can use the sizing function Rate (or ) to control how rapidly the cell size varies from the

boundary. The value of  should be specified such that

. A positive value indicates

a slower transition from the boundary to the specified sizing function Variation value. Conversely,

a negative value indicates a faster transition from the boundary to the sizing function Variation

value. A value of  indicates a linear variation of cell size away from the boundary.

You can also control the Resolution of the sizing function. This determines the size of the background

bins used to evaluate the size distribution with respect to the shortest feature length of the current

mesh. By default, the sizing function Resolution is  in 2D problems, and  in 3D problems.

Note that if you edit the Resolution, Variation, and/or Rate, clicking Default will return these fields

to the default values based on the current mesh. The Default button will then change to be a Reset

button, which can be used to return to the prior values.

In summary, the sizing function is a distance-weighted average of all mesh sizes on all boundary

faces (both stationary and moving boundaries). The sizing function is based on the sizes of the

boundary cells, with the size computed from the cell volume by assuming a perfect (equilateral)

triangle in 2D and a perfect tetrahedron in 3D. You can control the size distribution by specifying

the sizing function Variation and the sizing function Rate. If you have enabled the Sizing Function

option, ANSYS Fluent will agglomerate a cell if

(.)

where  is a factor defined by Equation . (p. ) and Equation . (p. ).

Note that the sizing function is only used for marking cells before remeshing. The sizing function is

not used to govern the size of the cell during remeshing.

For steady-state applications (see Steady-State Dynamic Mesh Applications (p. )), you can instruct

ANSYS Fluent to perform a second round of cell marking and agglomeration after the boundary has

moved, based on skewness criteria. The intent is to further improve the mesh quality through addi-

tional local remeshing. This optional feature works in conjunction with the Mesh Method Settings

dialog box (Figure . : The Remeshing Tab in the Mesh Method Settings Dialog Box (p. )), and

operates according to the skewness parameters you set in this dialog box. The sizing function

parameters are not considered during this additional remeshing. Note that enabling this option will

increase the time required to update the mesh during the solution.

Note

If you want to employ additional local remeshing, first make sure that you have enabled

the Remeshing option in the Dynamic Mesh Task Page (p. ).

To enable the additional round of local remeshing, use the following text command:

define → dynamic-mesh → controls → remeshing-parameter → remeshing-after-

moving?

..... Cell Zone Remeshing Method

The cell zone remeshing method allows for the remeshing of the complete cell zone, and provides

moving?

the option to also remesh the faces of all adjacent deforming dynamic face zones. This remeshing

method is enabled by default when local cell remeshing is enabled, and is performed automatically

if the local cell remeshing does not produce an acceptable mesh (see Local Remeshing Method (p. )

for the acceptability criteria). Cell zone remeshing can also be manually invoked, using the following

define → dynamic-mesh → actions → remesh-cell-zone

The cell zone remeshing method is available for triangular cells in 2D meshes and tetrahedral cells

in 3D meshes. For 3D meshes, the method also allows the remeshing of wedge cells in boundary

layers. The detection of the boundary layers (as well as the wedge element height distribution and

number of layers) is automatically performed by default, and allows for different layer parameters

on each boundary zone. You can manually specify the parameters by entering nonzero values for

first height, growth rate, and number of layers via the text commands available in the

define/dynamic-mesh/controls/remeshing-parameters/prism-layer-parameters

menu, although generally it is not necessary to do this. When you enter them manually, the

boundary layer parameters are global: they apply to every prism layer detected in the remeshing

zone.

Note that it is necessary to enable the dynamic mesh model and the remeshing method in order to

attain access to the prism layer controls, even if the cell zone is remeshed manually and not as part

of a dynamic mesh update.

...... Limitations of the Cell Zone Remeshing Method

Zone remeshing has the following limitations:

Only triangular, tetrahedral, and wedge cell types (when the wedge cells are part of a 3D boundary layer

mesh) are remeshed.

Zones with hanging nodes cannot be remeshed.

..... Face Region Remeshing Method

The face region remeshing method allows for the remeshing of those triangular faces (in 3D meshes)

and linear faces (in 2D meshes) that are on a deforming face zone and adjacent to a moving face

zone (see layer j in Figure . : Expanding Cylinder Before Region Face Remeshing (p. )). ANSYS

Fluent marks the faces based on minimum and maximum length scales, and then remeshes the faces

and the associated cells to produce a very regular mesh on the deforming boundary. Although

primarily designed for in-cylinder type configurations, where the remeshing region is located where

cylinder walls meet the moving piston, face region remeshing can be used for all applications where

a moving dynamic zone abuts deforming dynamic face zones.

For 3D simulations, ANSYS Fluent allows face region remeshing with symmetric boundary conditions

and across multiple face zones. The remeshing can preserve features not only between the different

deforming face zones, but also within a face zone. For more information on feature preservation,

see Feature Detection (p. ). ANSYS Fluent also allows face region remeshing of tetrahedral cell

zones that contain wedge cells in boundary layers, as described in the section that follows.

To begin marking the faces for face region remeshing, ANSYS Fluent identifies the nodes at the in-

tersection of a moving dynamic zone and the adjacent deforming zones. ANSYS Fluent then analyzes

the height of the faces on the deforming zones that are in the range of the identified nodes, and

then remeshes the faces depending on the specified maximum or minimum length scale.

Consider the simple tetrahedral mesh of a cylinder that has a moving end wall (see Figure . : Ex-

panding Cylinder Before Region Face Remeshing (p. )). The faces that are subject to remeshing

are in layer j of the side wall. If the faces in layer j are expanding, the expansion continues until the

height h reaches the maximum length scale, and then the layer is remeshed to form  layers of

elements (see Figure . : Expanding Cylinder After Region Face Remeshing (p. )). Conversely, if

the faces of layer j are contracting, the contraction continues until h reaches the minimum length

scale, and then layer j and the neighboring layer of faces (layer i) on the deforming zone are remeshed

to form a single layer.

Figure . : Expanding Cylinder Before Region Face Remeshing

Figure . : Expanding Cylinder After Region Face Remeshing

...... Face Region Remeshing with Wedge Cells in Prism Layers

In 3D simulations, the face region remeshing method can be applied on meshes that have wedge

cells along the deforming face zones. When remeshing the faces on the deforming face zones, the

associated wedge cells are remeshed as well. The layer parameters are based on the existing mesh

by default; you have the option of manually setting these parameters, as described later in this

section.

If the motion of the face zone is large compared to the height of the adjacent deforming face zones,

it is recommended that you decompose the mesh volume in such a way as to create a dynamic cell

zone that moves as a rigid body in between the moving face zone and the deforming dynamic cell

zone on which face region remeshing is applied. Consider Figure . : Volume Decomposition for

Prism Layers (p. ), which displays only half of an in-cylinder mesh. The rigidly moving cell zone

encapsulates the prism layers on the moving piston so that the layers are not remeshed, and

therefore the risk of generating degenerate cells during the mesh motion update is reduced.

Figure . : Volume Decomposition for Prism Layers

It is preferable (and even mandatory, if the mesh is a half model with a symmetry plane) to decompose

the volume such that the “corner” region of the prism layers (shown in the previous figure) exists

entirely within the rigidly moving zone. This allows for the largest deformations without risking de-

generate elements, because the prism normals of the remeshed cells are uniformly perpendicular

to the faces undergoing remeshing.

If the range of motion does not allow you to encapsulate the entire corner region of the prism layers

in a rigidly moving zone, it is recommended that you encapsulate the “base” of the prism layers

(shown in Figure . : Volume Decomposition for the Base of the Prism Layers (p. )) and move

these cells with a rigid body motion. Although this is less ideal than encapsulating the corner region,

it does reduce the risk of degenerate mesh elements.

Figure . : Volume Decomposition for the Base of the Prism Layers

For piston-type applications that contain prism layers, a reasonable rule of thumb is that you should

decompose the mesh volume if the piston motion is more than half the cylinder height. If you decide

not to decompose the volume at all, you must at the very least enable the Deform Adjacent

Boundary Layer with Zone option in the Meshing Options tab of the Dynamic Mesh Zone dialog

box when setting up the moving face zone (see Rigid Body Motion (p. ) for details). In any case,

it is recommended that you always preview the mesh motion over the complete simulation time,

to make sure that you will have a valid mesh at each time step.

The prism layer parameters (that is, element height, growth rate, and number of layers) are extracted

automatically from the mesh and do not generally require your input. To prevent the prism parameters

from drifting due to repeated remeshing, the prism parameters for first height, growth rate, and

number of layers can be entered manually, using the text commands available in the define/dy-

namic-mesh/controls/remeshing-parameters/prism-layer-parameters menu.

...... Applicability of the Face Region Remeshing Method

Note the following limitations associated with face region remeshing:

You can use the face region remeshing method only in cell zones that contain triangular cells (in 2D) or

tetrahedral cells, with or without prism layers (in 3D). For 3D meshes, the faces on the deforming

boundaries that border the moving face must all be triangular.

The face region remeshing method is not compatible with diffusion-based smoothing or linearly elastic

solid smoothing.

You cannot use the face region remeshing method in conjunction with adaption. For more information

on the available adaption methods, see Hanging Node Adaption and Polyhedral Unstructured Mesh

Adaption in the Theory Guide.

..... CutCell Zone Remeshing Method

The CutCell zone remeshing method is available to remesh a complete cell zone (including all

boundary zones of the remeshed cell zone). This method is available for 3D simulations only. The

existing volume mesh is replaced by a predominantly Cartesian mesh. Inflation layers can be added

as an option. When used as part of a transient simulation, the remeshing occurs at predefined intervals

and whenever the mesh quality in the cell zone is deemed poor. Examples of meshes before and

after CutCell zone remeshing are shown in Figure . : Unstructured Tetrahedral Mesh Before CutCell

Zone Remeshing (p. ) and Figure . : Mesh After CutCell Zone Remeshing (p. ), respectively.

Figure . : CutCell Zone Remeshing With Inflation Layers (p. ) shows a cut through a CutCell

mesh with inflation layers.

Figure . : Unstructured Tetrahedral Mesh Before CutCell Zone Remeshing

Figure . : Mesh After CutCell Zone Remeshing

Figure . : CutCell Zone Remeshing With Inflation Layers

During CutCell zone remeshing, a uniform Cartesian grid is locally refined using size functions, in

order to resolve the initial mesh with sufficient accuracy. The resulting mesh consists mostly of

hexahedral elements, which reduces the cell count compared to unstructured tetrahedral meshing.

Additional element types are used near the boundaries to closely resolve complex shapes. The

remeshing takes place at regular intervals, or whenever the mesh quality deteriorates due to mesh

motion.

The CutCell zone remeshing method not only replaces the volume mesh, it also replaces the complete

surface mesh of the remeshed cell zone. Consequently, this method can only be used to remesh cell

zones that are either stand-alone zones or are only connected to other cell zones through non-

conformal interfaces. If inflation layers are added to a CutCell mesh, the inflation layers are grown

from the remeshed surface mesh, and the CutCell mesh is morphed such that it smoothly matches

the cap surfaces of the inflation layers.

The CutCell Zone remeshing method option is available in the Remeshing Methods group box.

Note that the CutCell Zone remeshing method does not use any of the parameters specified in the

Mesh Method Settings dialog box. The parameters used to control CutCell Zone remeshing are

specified in the Dynamic Mesh Zones dialog box when setting up the zone and boundaries.

For more information about CutCell meshes, see Generating the CutCell Mesh (p. ) in the Fluent

Meshing section of the User’s Guide.

...... Applicability of the CutCell Zone Remeshing Method

The CutCell zone remeshing method can be applied to cell zones, with the following limitations:

The case must be 3D.

The cell zone cannot be conformally connected to other cell zones; that is, a CutCell zone must be a

stand-alone cell zone, or can only be connected to another zone through a non-conformal interface. In

the latter case, the non-conformal interface is cleared before the remeshing and automatically recreated

after the remeshing.

Note that the CutCell zone remeshing method can be applied to cell zones that contain adapted

cells.

In parallel, all cells of the remeshed zone will be automatically migrated to and remeshed on a single

CPU. Consequently, the machine memory will limit the size of the zone that can be remeshed. The

mesh is automatically repartitioned after the remeshing.

In addition to the limitations listed previously, you should also note the following with regard to

CutCell zone remeshing:

Internal coupled walls, such as baffles, are discarded during the remeshing.The method is designed

to primarily remesh cell zones with a single interior zone.

Interior jump boundary condition zones (for example, fans, porous jumps), are discarded during the

remeshing.

Conformal periodic boundary conditions are not maintained after the remeshing. Any existing

conformal periodic boundaries on the zone being remeshed should slit and replaced with non-

conformal periodic boundaries.

If the zone being remeshed contains multiple interior zones prior to the remeshing, all interior zones

will be collected into a single interior zone during the CutCell zone remeshing.

...... Using the CutCell Zone Remeshing Method

In order to apply CutCell zone remeshing to a cell zone, begin by enabling the CutCell Zone option

in the Remeshing Methods group box in the Remeshing tab of the Mesh Method Settings dialog

box (see Figure . : The Remeshing Tab in the Mesh Method Settings Dialog Box (p. )). Next,

use the Dynamic Mesh Zones dialog box to create a deforming dynamic zone for the cell zone (see

Deforming Motion (p. )). Then enable CutCell in the Remeshing Options group box and enter

the relevant remeshing parameters, including: the maximum mesh size for the Cartesian cells; the

global size function growth rate; the minimum orthogonal quality and remeshing interval to control

the remeshing frequency; and the optional global inflation layer settings.

ANSYS Fluent allows you to specify either a soft or a mesh-based size function to control how the

Cartesian mesh increases in size from the boundary toward the interior of the cell zone. For the soft

size function, you specify a maximum mesh size for each boundary zone of the CutCell cell zone.

When you use the mesh-based size function, ANSYS Fluent analyzes the existing mesh to evaluate

the necessary mesh refinement at the boundary. See step  of Stationary Zones (p. ) for more in-

formation about these size functions. You have control over the size function types and parameters

by defining the boundary zones as dynamic zones. If no boundary zone adjacent to the CutCell zone

is defined as a dynamic zone, ANSYS Fluent will automatically apply mesh-based size functions to

each CutCell boundary zone and use the global growth rate entered for the cell zone to control the

Note that the size functions used by the CutCell zone remeshing method are unrelated to the sizing

function used for local cell remeshing (as described in Local Remeshing Based on Sizing Func-

ANSYS Fluent allows you to add inflation layers to a CutCell mesh in order to better resolve wall-

bounded flow features. After enabling Inflation Layers under the CutCell Zone Parameters for the

CutCell cell zone, you can specify the global inflation parameters in the Inflation Settings dialog

box. There are two types of inflation layers available: a constant type, where you can specify the

constant height of the first layer; and an aspect-ratio type, where the first layer height is locally

evaluated based on the specified aspect ratio. The latter is recommended and used by default since

it is more robust and generally produces higher quality CutCell meshes. By default, the inflation

settings specified apply to every boundary of the cell zone. If you would like to specify different in-

flation settings for different boundaries, you can define these boundaries as dynamic zones and

enable Zonal Inflation Layer Control. Note that the Number of Layers, other than , has to be the

same on all boundary zones. If different numbers of layers are specified on different boundaries,

ANSYS Fluent will only inflate up to the largest common number specified. By setting the number

of layers on a boundary zone to , you can locally suppress the growth of inflation layers, however,

note that the transition is handled by stair stepping and adding wedge elements, which tends to

generate skewed elements for small layer element heights.

The cells that contain hanging nodes / edges as a result of the CutCell zone remeshing are automat-

ically converted to polyhedral cells. See Limitations (p. ) for details about limitations associated

with polyhedral cells.

It is recommended that you first manually apply the CutCell zone remeshing method (as described

in the section that follows) and inspect the mesh before using the method as part of a transient

simulation, as this allows you to evaluate if your remeshing parameters are suitable before running

a calculation that is computationally expensive.

...... Applying the CutCell Zone Remeshing Method Manually

Although the CutCell zone remeshing method is primarily intended as an automatic remeshing

method during dynamic mesh updates, you can also manually create a CutCell mesh (that is, you

can remesh without running a calculation) by using the following text command:

define → dynamic-mesh → actions → remesh-cell-zone-cutcell

You will be prompted to enter the global parameters for the CutCell zone remeshing. If no dynamic

zones are set up in your case, ANSYS Fluent will use the global parameters you enter and apply

mesh-based size functions to each boundary of the CutCell zone. If the case is set up as a dynamic

mesh case, manual remeshing will use the information specified on each CutCell boundary zone,

including the zonal inflation layer settings. During manual CutCell zone remeshing, the global

parameters are taken from the text interface input, and the global parameters specified on the

CutCell cell zone are ignored.

When executing manual remeshing through the remesh-cell-zone-cutcell text command,

you will be prompted to specify whether topology warnings should be ignored. If you do not ignore

the topology warnings, ANSYS Fluent will analyze the zone being remeshed and report any interior

face zones that will get discarded during the remeshing. If the zone being remeshed has periodic

boundary zones, you will also be prompted to either abort the remeshing process or slit the periodics

in order to proceed.

You will also be prompted to specify whether the cells that contain hanging nodes / edges as a

result of the CutCell zone remeshing should be converted to polyhedral cells. See Limitations (p. )

for details about limitations associated with polyhedral cells. By default, all hanging node cells are

converted to polyhedral cells.

..... .5D Surface Remeshing Method

The .5D surface remeshing method only applies to extruded 3D geometries and is similar to local

remeshing in two dimensions on a triangular surface mesh (not a mixed zone). Faces on a deforming

boundary are marked for remeshing based on face skewness, minimum and maximum length scale;

the .5D remeshing method also gives you the option of marking cells using sizing functions, as

described in Local Remeshing Based on Sizing Function (p. ).

Figure . : Close-Up of .5D Extruded Flow Meter Pump Geometry Before Remeshing and

Laplacian Smoothing

Figure . : Close-Up of .5D Extruded Flow Meter Pump Geometry After Remeshing and

...... Applicability of the .5D Surface Remeshing Method

The following applies to the .5D surface remeshing method:

Triangular faces get remeshed based on marking.

Extruded wedges get remeshed based on the remeshing of the triangular face. Only extruded regions

get remeshed, not mixed regions.

The .5D remeshing method does not support remeshing or moving nodes on the perimeter of the ex-

truded zone(s).

Note that you cannot use the .5D surface remeshing method in conjunction with adaption. For more

information on the available adaption methods, see Hanging Node Adaption and Polyhedral Unstructured

Mesh Adaption in the Theory Guide.

The extrusion must be along a straight line normal to the deforming zone and the cross-section of the

extruded/coopered mesh must be constant along the extrusion direction. For more information about

the .5D model, see Using the .5D Model (p. ).

Periodics are not supported at the extruded zones.

...... Using the .5D Model

For 3D simulations only, you can select the .5D model under the Remeshing tab in the Mesh

Method Settings Dialog Box (p. ). This model allows for a specific subset of remeshing techniques.

The .5D mesh essentially is a 2D triangular mesh which is expanded, or extruded, along the normal

axis of the specific dynamic zone that you are interested in modeling. The triangular surface mesh

is remeshed and smoothed on one side, and the changes are then extruded to the opposite side.

Rigid body motion is applied to the moving face zones, while the triangular extrusion surface is as-

signed to a deforming zone with remeshing and smoothing enabled. The opposite side of the trian-

gular mesh is assigned to be a deforming zone as well, with only smoothing enabled, as in Fig-

ure . : .5D Extruded Gear Pump Geometry (p. ).

Figure . : The Remeshing Tab for the .5D Model

For more information on setting smoothing and remeshing parameters, see Dynamic Mesh Update

Methods (p. ).

The .5D model only applies to mappable (that is, extrudable) mesh geometries such as pumps, as

in Figure . : .5D Extruded Gear Pump Geometry (p. ). Only the aspects of the geometry that

represent the “moving parts” must be extruded in the mesh.

Figure . : .5D Extruded Gear Pump Geometry

Important

You must only apply smoothing to the opposite side of the extruded mesh, since ANSYS

Fluent requires the geometry information for the dynamic zone. ANSYS Fluent projects

the nodes back to its geometry after the extrusion. Without this geometry information,

the dynamic zones tends to lose its integrity.

Important

Important

In parallel, a partition method that partitions perpendicular to the extrusion surface should

be used. For example, if the normal of the extrusion surface points in the X-direction then

Cartesian-Y or Cartesian-Z would be the perfect partition methods.

The .5D model is used in combination with a DEFINE_GRID_MOTION UDF. (See Hooking

DEFINE_GRID_MOTION UDFs in the Fluent Customization Manual for information about hooking

this UDF.)

This UDF is associated with the extrusion surface that is adjacent to the cell zone, in turn applying

the same deformation to the entire cell zone. This approach is particularly useful when modeling

gear pumps that are predominantly extruded hexahedral meshes. For more information about this

UDF, contact your support engineer.

....Volume Mesh Update Procedure

The volume mesh is updated automatically based on the methods described in Dynamic Mesh Update

Methods (p. ). ANSYS Fluent decides which method to use for a particular zone based on which

model is enabled and the shape of the cells in the zone. For example, if the boundaries of a tetrahedral

cell zone are moving, and unless the zone has been set up for CutCell zone remeshing, the mesh

smoothing and local remeshing methods will be used to update the volume mesh in this zone. If the

zone consists of prismatic (hexahedral and/or wedge) cells, then the dynamic layer method will be

used to determine where and when to insert and remove cell layers. On extruded prism zones, the

.5D surface meshing method will be used.

Depending on which model is enabled, ANSYS Fluent automatically determines which method to use

by visiting the adjacent cell zones and setting appropriate flags for the volume mesh update methods

to be used. If you specify the motion for a cell zone, ANSYS Fluent will visit all of the neighboring cell

zones and set the flags appropriately. If you specify the motion of a boundary zone, ANSYS Fluent will

analyze only the adjacent cell zones. If a cell zone does not have any moving boundaries, then no

volume mesh update method will be applied to the zone.

Important

Note that as a result of the remeshing procedures, updated meshes may be slightly different

when dynamic meshes are used in parallel ANSYS Fluent, and therefore very small differ-

ences may arise in the solutions.

Important

Note that if your dynamic mesh model consists of numerous shell conduction zones, the

mesh update may be very time consuming because all shells are deleted and recreated

during the mesh update.

....Transient Considerations for Remeshing and Layering

The second order in time transient formulation can be used with remeshing, layering, and smoothing

cases. In such cases, second order in time accuracy is preserved during layering events and/or mesh

smoothing. However, during remeshing events, the time advancement accuracy reverts to first order.

Therefore, it is recommended that you only use second order in time for cases with very low

remeshing frequency, that is, for cases where remeshing occurs every several timesteps or more. If

remeshing occurs every timestep, the method reduces to a first order formulation. For cases that

need very frequent remeshing, it is recommended that you retain the first order in time formulation.

For details, see Dynamic Mesh Theory in the Fluent Theory Guide.

The switch to first order happens automatically when the solver detects a topology change as a result

of remeshing within a timestep. You will not see a change in the user interface, however you can

monitor the switch between first and second order in time by using the following text command to

enable the verbosity with dynamic meshes:

define → dynamic-mesh → transient-settings → verbosity

A message showing the active time formulation will print to the console when verbosity is set to .

Note

For cases with second order in time with dynamic mesh enabled, any mesh swapping and

manual mesh manipulation will trigger a switch to first order in time.

The remeshing and/or smoothing of boundary zones may result in the chamfering of corners where

cell faces meet. However, there may be some corners (identified by a particular angular range) that

are important for your flow, and that you do not want chamfered. For 3D cases, you can specify that

ANSYS Fluent detects such corners (or "features") and preserves them. Such features may be at the

juncture of different boundary zones, or they may be on a single non-planar boundary zone.

In the Geometry Definition tab of the Dynamic Mesh Zones Dialog Box (p. ) for any Definition

type, you can indicate whether you want to preserve features by enabling Feature Detection under

Feature Options and specifying a threshold value for the Feature Angle. A value of  degrees (the

default) for the Feature Angle means that none of the corners must be preserved, whereas a value

of  means that all of the corners must be preserved.

To illustrate the setting of the Feature Angle, see Figure . : Cross Section of a 3D Corner (p. ).

If you set the Feature Angle to  degrees, this corner would be guaranteed to be preserved. If you

set it to  degrees, this corner could be chamfered.

Figure . : Cross Section of a 3D Corner

.... Applicability of Feature Detection

The following items are applicable for use with feature detection:

Feature remeshing is only possible with face region remeshing.

Features are preserved by local face remeshing, that is, there is no local face remeshing across features.

Smoothing methods preserve features, that is, nodes at feature edges are not allowed to be smoothed.

You can enable the In-Cylinder option in the Dynamic Mesh Task Page (p. ) (Figure . : The Dy-

namic Mesh Task Page (p. )) for transient problems. Then click the Settings... button in the Options

group box to open the Options Dialog Box (p. ). Click the In-Cylinder tab and specify the Crank

Shaft Speed, the Starting Crank Angle, and the Crank Period, which are used to convert between

flow time and crank angle. You must also specify the time step to use for advancing the solution in

terms of crank angle in Crank Angle Step Size. By default, ANSYS Fluent assumes a Crank Angle Step

Size of . degrees.

Figure . : The In-Cylinder Tab of the Options Dialog Box

ANSYS Fluent provides a built-in function that can define the location of the piston as a function of

crank angle. This function is named **piston-full**, and is selected from the Motion/UDF Profile

drop-down list in the Dynamic Mesh Zones dialog box as part of rigid body motion (see Rigid Body

Motion (p. ) for details). If you plan to specify the piston motion using this function, you must specify

the Crank Radius (that is, the distance between the crank center and the center of the crank pin) and

the Connecting Rod Length. You also have the option of entering a value for the Piston Pin Offset

for cases when the piston pin is offset perpendicularly from the plane defined by the crank shaft axis

and the direction of motion of the piston. The sign of this offset can be positive or negative, and is

determined based on the geometry and the direction of rotation of the crank shaft (as shown in Fig-

ure . : Determining the Sign of the Piston Pin Offset (p. )).

Figure . : Determining the Sign of the Piston Pin Offset

When the **piston-full** function is used, the piston location is calculated according to the following

equation:

(.)

where

is the piston location,

the crank radius,

is the connecting rod length,

is the piston

pin offset, and

is the current crank angle.

The piston location

is always  at top-dead-center (TDC), that is, when the crank pin is perfectly

aligned between the piston pin and the center of rotation of the crank shaft. TDC occurs when the

crank angle is ° when there is no piston pin offset, and prior to the crank angle reaching ° when

there is a positive piston pin offset. The piston location is a positive value at bottom-dead-center (BDC),

that is, when the crank shaft is perfectly aligned between the piston pin and the crank pin. The value

of

at BDC is equal to

when there is no piston pin offset, and greater than

when there is a

nonzero piston pin offset (positive or negative).

The current crank angle

is calculated from

(.)

where

is the Starting Crank Angle and

is the Crank Shaft Speed.

The Piston Stroke Cutoff and Minimum Valve Lift values are used to control the actual values of the

valve lift and piston stroke such that

(.)

where

is the valve lift computed from the appropriate valve profiles,

is the Minimum Valve

Lift,

is the stroke calculated from Equation . (p. ), and

is the Piston Stroke Cutoff. (See

Defining Motion/Geometry Attributes of Mesh Zones (p. ) on how the Piston Stroke Cutoff is used

to control the onset of layering in the cylinder chamber.)

Enable the Write In-Cylinder Output option then click the Output Controls... button if you want to

specify specific output parameters. The In-Cylinder Output Controls Dialog Box (p. ) will open, where

you can specify various quantities needed for the calculation of swirl and tumble along with the fre-

quency of writing the output to the chosen file. Swirl is used to describe circulation about the cylinder

axis. Tumble flow circulates around an axis perpendicular to the cylinder axis, orthogonal to swirl flow.

Figure . : The In-Cylinder Output Controls Dialog Box

The following list describes the In-Cylinder Output Controls Dialog Box (p. ).

In-Cylinder Data Write Frequency

is an integer entry specifying the interval in number of time-steps. Make sure that a value other than  is

used for the frequency, in order to allow you to complete your setup.

Swirl Center Method

is a drop-down list that allows you to select the method to calculate the swirl center.The list contains

center of gravity and fixed, with center of gravity being the default value.

center of gravity

option calculates the swirl center inside the code and is used as the center of gravity of the chosen

cell zones.

fixed

option enables you to specify a swirl center in the entries below the drop-down list.

In addition to these two options, you can chose to use your own compiled UDF to calculate the

swirl center.

For details on using a dynamic mesh UDF, see the Fluent Customization Manual for information

on user-defined functions.

Cell Zones

is a list that displays the names of all existing cell zones in the case files.You can select only the zones

relevant for the swirl and tumble calculations.

Swirl Axis

specifies the swirl axis with three entries for the directional components. By default, X, Y, Z = , , .

Tumble Axis

specifies the directional components of Tumble Axis in X, Y, Z directions. By default, X, Y, Z = , , .This

applies only in 3D.

Cross Tumble Axis

specifies the directional components of Cross Tumble Axis in X, Y, Z directions. By default, X, Y, Z = ,

, .This applies only in 3D.

File Name

specifies the name of the In-Cylinder output file. By default, the file name contains the name of the case

file appended with a .txt extension.

The In-Cylinder specific output controls can also be controlled using the TUI as follows:

Go to

define/dynamic-mesh/controls/in-cylinder-output?

Enable in-cylinder output? [no] yes

Output Write Frequency[]

Cell zone name/id()[()]

File Name[‘‘/nfs/devvault/data9/ic-sp-output.txt’’]

Swirl Center Method: (fixed cg user-defined)

Option[cg]

Swirl Axis x[]

Swirl Axis y[]

Swirl Axis z[]

Tumble Axis x[]

Tumble Axis y[]

Tumble Axis z[]

Cross Tumble Axis x[]

Cross Tumble Axis y[]

Cross Tumble Axis z[]

If you select fixed as the choice at Swirl Center Method then you will be prompted to enter the swirl

center as follows:

Swirl Center(x) (mm) []

Swirl Center(y) (mm) []

Swirl Center(z) (mm) []

If a swirl center method UDF has been compiled already and loaded into UDF then you can choose

user-defined as the swirl center method option, in such a case the following is the sequence of

prompts.

Swirl Center UDF[] swirl_udf::libudf

If the name of the UDF library is libudf then you can omit this and enter in the swirl center

UDF[]swirl_udf, otherwise the name of the UDF followed by the UDF library name with symbol::

in between, should be entered.

By filling up the various entries that are needed in the In-Cylinder Output Controls Dialog Box (p. )

and pressing the OK button, the swirl and tumble calculations will be written at the chosen frequency

to the chosen file while doing the solution run. Details of the quantities written to the file are as follows:

CA = Crank Angle

m = Mass of the entire fluid contained in the selected cell zones

L = Angular momentum vector of fluid mass contained in selected cell zones with respect to the

swirl center

= Magnitude of angular momentum of fluid

= Swirl Axis

= Tumble Axis

= Cross Tumble Axis

I

= Moment of inertia of the fluid mass about Swirl axis

I

= Moment of inertia of the fluid mass about Tumble Axis

I

= Moment of inertia of the fluid mass about Cross Tumble Axis

= Dot product between two vectors

Altogether, the previous quantities are combined to yield eight columns of data in the output file, as

shown in the figure that follows:

Figure . : Sample Output File Showing Various Quantities

.... Using the In-Cylinder Option

This section describes the problem setup procedure for an in-cylinder dynamic mesh simulation.

..... Overview

Consider the 2D in-cylinder example shown in Figure . : A 2D In-Cylinder Geometry (p. ) for

a typical pent-roof engine.

Figure . : A 2D In-Cylinder Geometry

In setting up the dynamic mesh model for an in-cylinder problem, you must consider the following

issues:

how to provide the proper mesh topology for the volume mesh update methods (smoothing, dynamic

layering, and local or zonal remeshing)

how to define the motion attributes and geometry for the valve and piston surfaces

how to address the opening and closing of the intake and exhaust valves

how to specify the sequence of events that controls the in-cylinder simulation

..... Defining the Mesh Topology

ANSYS Fluent requires that you provide an initial volume mesh with the appropriate mesh topology

such that the various mesh update methods described in Dynamic Mesh Update Methods (p. )

can be used to automatically update the dynamic mesh. However, ANSYS Fluent does not require

you to set up all in-cylinder problems using the same mesh topology. When you generate the mesh

for your in-cylinder problem, you must consider the various mesh regions that you can identify as

moving, deforming, or stationary, and generate these mesh regions with the appropriate cell shape.

The mesh topology for the example problem in Figure . : A 2D In-Cylinder Geometry (p. ) is

shown in Figure . : Mesh Topology Showing the Various Mesh Regions (p. ), and the corres-

ponding volume mesh is shown in Figure . : Mesh Associated With the Chosen Topology (p. ).

Figure . : Mesh Topology Showing the Various Mesh Regions

Figure . : Mesh Associated With the Chosen Topology

Because of the rectilinear motion of the moving surfaces, you can use dynamic layering zones to

represent the mesh regions swept out by the moving surfaces. These regions are the regions above

the top surfaces of the intake and exhaust valves and above the piston head surface, and must be

meshed with quadrilateral or hexahedral cells (as required by the dynamic layering method).

For the chamber region, you must define a remeshing zone (triangular cells) to accommodate the

various positions of the valves in the course of the simulation. In this region, the motion of the

boundaries (valves and piston surfaces) is propagated to the interior nodes through smoothing. If

the cell quality violates any of the remeshing criteria that you have specified, ANSYS Fluent will

automatically agglomerate these cells and remesh them. Furthermore, ANSYS Fluent will also remesh

the deforming faces (based on the minimum and maximum length scale that you have specified)

on the cylinder walls as well as those on the sliding interfaces used to connect the chamber cell

zone to the layering zones above the valve surfaces.

For the intake and exhaust port regions, you can use either triangular or quadrilateral cell zones

because these zones are not moving or deforming. ANSYS Fluent will automatically mark these regions

as stationary zones and will not apply any mesh motion method on these cell zones.

The dynamic layering regions above the piston and valves are conformal with the adjacent cell zone

in the chamber and ports, respectively, so you do not have to use sliding interfaces to connect these

cell zones together. However, you must use sliding interfaces to connect the dynamic layering regions

above the valves and the remeshing region in the chamber. This is shown in Figure . : The Use

of Sliding Interfaces to Connect the Exhaust Valve Layering Zone to the Remeshing Zone (p. )

with the exhaust valve almost at full extension. Notice that cells on the chamber side of the interface

zone are remeshed (that is, split or merged) as the interface zone opens and closes because of the

motion of the exhaust valve.

Figure . : The Use of Sliding Interfaces to Connect the Exhaust Valve Layering Zone to the

Remeshing Zone

..... Defining Motion/Geometry Attributes of Mesh Zones

As the piston moves down from the TDC to the BDC position, you must expand the remeshing region

such that it can accommodate the valves when they are fully extended. To accomplish this, you

must specify the dynamic layering zone adjacent to the piston surface to move with the piston until

some specified distance from the TDC position. Beyond this cutoff distance, the motion of the layering

zone is stopped and the piston wall is allowed to continue to the BDC position. Because there is

relative motion between the piston head surface and the now non-moving dynamic layering zone,

cell layers will be added when the ideal layer height criteria is violated. Figure . : Mesh Sequence

(p. ) to Figure . : Mesh Sequence  (p. ) show the sequence of meshes before and after

the onset of cell layering when the motion in the layering zone above the piston surface is stopped

(shown with

= °).

Figure . : Mesh Sequence

ANSYS Fluent provides built-in functions to handle the full piston motion and the limited piston

motion for the dynamic layering zone above the piston surface. When you define the motion attribute

of the dynamic layering zone above the piston surface, you must use the limited piston motion

function (**piston-limit** in the Motion UDF/Profile field in the Dynamic Mesh Zones Dialog

Box (p. )). Note that you must define the parameters used by these functions before you can use

them. In the current example, the crank radius is  mm and the connecting rod length is  mm.

The piston stroke cutoff is assumed to happen at  mm from TDC position. The lift as a function

of crank angle between

and

is shown in Figure . : Piston Position (m) as a Function

of Crank Angle (deg) (p. ) for both limited and full piston motion.

Figure . : Piston Position (m) as a Function of Crank Angle (deg)

To define the motion of the valves, you must use profiles that describe the variation of valve lift

with crank angle. ANSYS Fluent expects certain profile fields to be used to define the lift and the

crank angle. For example, consider the following simplified profile definition:

((ex-valve  point)

(angle       )

(lift . . . . .))

((in-valve  point)

(angle       )

ANSYS Fluent expects the angle and lift fields to define the crank angle and lift variations, re-

spectively. The angle must be specified in degrees and the lift values must be in meters. The actual

valve lift profiles that you will use for the current example are shown in Figure . : Intake and

Exhaust Valve Lift (m) as a Function of Crank Angle (deg) (p. ). Notice that there is an overlapped

period where both the intake and exhaust valves are open.

Figure . : Intake and Exhaust Valve Lift (m) as a Function of Crank Angle (deg)

The valve lift profiles and the built-in functions will describe how each surface moves as a function

of crank angle with respect to some reference point. For example, the valve lift is zero when the

valve is fully closed and the valve lift is maximum when it is fully open. In order to move the surfaces,

ANSYS Fluent requires that you specify the direction of motion for each surface. ANSYS Fluent will

then update the “center of gravity” of each surface such that

(.)

where

is some reference position,

is the unit vector in the direction of motion, and  is

either the valve or the piston distance with respect to the reference position

. Note that the unit

vector of the direction of motion is specified to point in the negative direction. For example, the

correct intake valve axis for this example is

, as shown in Figure . : Definition

of Valve Zone Attributes (Intake Valve) (p. ).

Figure . : Definition of Valve Zone Attributes (Intake Valve)

..... Defining Valve Opening and Closure

ANSYS Fluent assumes that once you have set up the mesh topology, the mesh topology is unchanged

throughout the entire simulation. Therefore, ANSYS Fluent does not allow you to completely close

the valves such that the cells between the valve and the valve seat become degenerate (flat cells)

when these surfaces come in contact (removing these flat cells would require the creation of new

boundary face zones). To prevent the collapse, you must define a minimum valve lift and ANSYS

Fluent will automatically stop the motion of the valve when the valve lift is smaller than the minimum

valve lift value. The minimum valve lift value can be specified in the In-Cylinder tab of the Options

Dialog Box (p. ). For the current example, a minimum valve lift value of . mm is assumed.

When the valve position is smaller than the minimum valve lift value, it is normal practice to assume

that the valve is closed. The actual closing of the valves is accomplished by deleting the sliding in-

terfaces that connect the chamber cell zone to the dynamic layering zones on the valves. The interface

zones are then converted to walls to close off the “gaps” between the valves and the valve seats.

The valve opening is achieved by the reverse process. When the valve lift has reached beyond the

minimum valve lift value, the valve is assumed to be open and you can redefine the sliding interfaces

such that the chamber zone is now connected to the dynamic layering zones above the valves.

ANSYS Fluent’s six degrees of freedom (six DOF) solver computes external forces and moments (such

as aerodynamic and gravitational forces and moments) on objects that undergo rigid body motion.

These forces are computed by numerical integration of pressure and shear stress over the object’s

surfaces. Additional load forces can be added, such as injector forces, thrust (propulsive) forces, and

moments produced by a coil spring. This technique, along with the ANSYS Fluent solver and the use

of dynamic meshes, can be readily applied to many useful applications, such as store separation

[] (p. ), [] (p. ). Note that the objects may be composed of multiple zones.

To use the six degrees of freedom solver for your transient dynamic mesh simulation, perform the

following steps:

. Enable the Six DOF option in the Options group box of the Dynamic Mesh Task Page (p. ) (Fig-

ure . :The Dynamic Mesh Task Page (p. )) and click the Settings... button.The Options dialog box

will open, where you can click the Six DOF tab (Figure . :The Six DOF Tab of the Options Dialog

Box (p. )).

Figure . : The Six DOF Tab of the Options Dialog Box

This tab allows you to perform the following actions:

You can create and manage sets of six DOF properties for rigid body motion by using the list and buttons

under Six DOF Properties; otherwise, you will have to create one or more user-defined functions. See

Setting Rigid Body Motion Attributes for the Six DOF Solver (p. ) for details.

You can specify the gravitational acceleration for the x, y, and z directions either in this dialog box, or

in the Operating Conditions dialog box.

You can keep track of an object’s motion history by enabling the Write Motion History option

and entering a File Name. A single motion history file will be generated for each moving object,

which can be used to display zone motion for postprocessing your results. Note that the file

name you specify will be appended with the name of the set of six DOF properties / UDF, as

well as the extension .6dof; you can change the extension by specifying your own as part of

the File Name.

. If the mesh motion of your six DOF simulation depends on the fluid flow, it is beneficial to enable implicit

mesh updating (as described in Implicit Update Settings (p. )). If the implicit mesh update is not sufficient

to stabilize the solver due to the fluid motion, solution stabilization may be necessary.The solution stabil-

ization settings are set in the Solver Options tab of the Dynamic Mesh Zones dialog box for boundary

zones (Solution Stabilization for Dynamic Mesh Boundary Zones (p. )).

. Define the rigid-body zone(s) that make up each moving object by using the Dynamic Mesh Zones Dialog

Box (p. ), as described in Rigid Body Motion (p. ).

Setup →

.... Setting Rigid Body Motion Attributes for the Six DOF Solver

As part of the six DOF solver settings, you must provide either a set of properties or a user-defined

function (UDF) for each moving object, in order to define its overall mass, rotational inertia, constraints,

loading from sources other than aerodynamics and gravity, and so on. Each object needs exactly one

set of properties / UDF, regardless of how many zones make up the object. Note that if you have

multiple identical objects, you can create an initial set of properties / UDF, and then make copies

with unique names.

If the motion of the object is complex or if only half of the object is modeled using a symmetry zone,

then you will need to use a UDF (see DEFINE_SDOF_PROPERTIES in the Fluent Customization

Manual for the details); otherwise, it is easier to use a set of properties. Such sets are created using

the Six DOF Properties dialog box, which is opened by clicking the Create/Edit... button in the Six

DOF tab of the Options Dialog Box (p. ).

Figure . : The Six DOF Properties Dialog Box

In the Six DOF Properties dialog box, you will need to provide a Name for the set of properties,

define the other fields in the dialog box, and click Create.

For six DOF motion, the only other fields that must be defined are the Mass and the Inertia Tensor

components. Note that the inertia tensor components are defined relative to the Center of Gravity

and Rigid Body Orientation settings defined in the Dynamic Mesh Zones Dialog Box (p. ); the

latter settings allow you to use a coordinate system that is local (rather than global), if that is more

convenient.

If you want to specify that the dynamic object be limited to one DOF motion (that is, either a simple

translation or a simple rotation), enable the One DOF Translation or One DOF Rotation option and

define the settings in the One DOF group box. The following figure shows an example of a one DOF

translation:

Figure . : A Check Valve with One DOF Translation

Note the following about one DOF motion settings:

For rotation, you will define the Mass of the dynamic object, in addition to the Moment of Inertia.

For 2D cases with rotation, the axis will be either the positive or negative z direction, depending on the

sign of the value you enter for Z in the Axis group box.

You have the option of defining a Hooke's law Spring that exerts forces / torques on the dynamic object.

It is a compression / extension spring for translations, and it is a torsion spring for rotations.

For example: for a translation, the specified Constant will be multiplied by the distance of the dy-

namic object from its initial location. This force will be combined with a Preload value that is

constantly applied to the dynamic object, in order to produce the net spring loading. Note that

the Preload can be a positive or negative value, and is defined relative to the Direction.

You can limit the range of motion of the dynamic object by enabling the Constrained option and defining

the settings in the Reference Point group box (for translation) or the Reference Angle group box (for

rotation).

For example: for a translation, you could enter  inches for the Location, in order to assign a co-

ordinate value to a point located on the dynamic object in its initial position. Then you would

define the range of motion allowed relative to that coordinate: you would enter . and  inches

for the Minimum and Maximum, respectively, if you wanted the object to only be allowed to move

. inches in the direction opposite to the Direction vector. The value of the Location is arbitrary,

and allows you to define the range using values that are most convenient for your problem.

The initial position / orientation of the object (which is used to calculate the spring loading and/or range

of motion) is established when you create the dynamic zone(s) using the Dynamic Mesh Zones Dialog

Box (p. ).

For transient problems, you can enable implicit mesh updating when you want to have the dynamic

mesh updated during a time step (as opposed to just at the beginning of a time step). This capability

is beneficial only for applications in which the mesh motion depends on the flow field (for example,

cases that use the six DOF solver or involve fluid-structure interaction). For such applications, having

the mesh motion updated within the time step based on the converging flow solution results in a

stronger coupling between the flow solution and the mesh motion, and leads to a more robust solver

run. Implicit mesh updating allows you to run simulations that otherwise could not be solved or would

require an unreasonably small time step.

Note that implicit mesh updating cannot be used with the following:

the density-based solver when Explicit is selected from the Transient Formulation drop-down menu

in the Solution Methods task page

steady-state solutions

in-cylinder applications

To enable implicit mesh updating, perform the following steps:

. Enable Implicit Update in the Options group box of the Dynamic Mesh Task Page (p. ) (Fig-

ure . :The Dynamic Mesh Task Page (p. )).

. Click the Settings... button to open the Options Dialog Box (p. ).

Figure . : The Implicit Update Tab of the Options Dialog Box

Click the Implicit Update tab and enter values for the settings.

a.

Enter a value for Update Interval, in order to specify the frequency in iterations at which

the mesh will be updated within a time step.

b. Enter a value (within the range of  to ) for Motion Relaxation, in order to define the

relaxation of the motion (that is, displacement of the nodes) during the mesh update. The

relaxation of the displacements is defined by the following equation:

(.)

where

is the node position at iteration  (within a time step),

is the

computed node position (based on the flow field), and

is the motion relaxation.

c.

Enter a value for Residual Criteria, in order to set the relative residual threshold that is

used to check the motion convergence. The residual criteria is applied to a relative residual.

ANSYS Fluent scales the difference between the motion in iteration  and iteration

by the motion computed at the beginning of the time step. If this relative motion difference

is smaller than the residual criteria, the mesh motion is considered converged.

. If you are using a UDF to compute the motion, make sure that the UDF uses the current flow field

during each call to compute the motion (that is, no previously stored information should be used).

This is necessary, as the UDF will be called each time the mesh is updated — which can be several

times within a time step, depending on what you entered for the Update Interval.

. After you run the simulation, make sure that the motion (and consequently, the solution) is properly

converged. If the motion requires more iterations to converge than the flow field, a warning will be

displayed in the console during the iteration process. Note that the maximum number of iterations

per time step (defined in the Run Calculation task page) is respected by the mesh motion convergence

check.

Contact detection is used to detect if the computed mesh motion will result in contact of a moving

surface with other surrounding surfaces. If there is contact within specified tolerances, then the mesh

motion of the moving zone can be constrained using nodal contact information within user-defined

functions (See Example  under DEFINE_CONTACT in the Fluent ).

To enable contact detection in your dynamic mesh simulation, select the Contact Detection check

box in the Options group of the Dynamic Mesh task page. Click the Settings... button to open the

Options dialog box and select the Contact Detection tab (see Figure . : The Contact Detection

Tab of the Options Dialog Box (p. )).

Figure . : The Contact Detection Tab of the Options Dialog Box

You can select the face zones that will be involved in the contact detection process from the Face

Zones list. While all eligible face zones in the Face Zones list are selected by default, you can choose

to exclude certain zones for efficiency. Only walls and dynamic zones of type Rigid Body or User-

Defined can be selected for contact detection.

From the UDF drop-down list, you can specify a user-defined function that will be invoked when

contact has been detected. For more information about contact UDFs, see DEFINE_CONTACT in the

Fluent Customization Manual.

You must specify a Proximity Threshold value in order to enable the contact detection process. When

the distance between face zones falls below this threshold value, the UDF specified in the UDF drop-

down list is invoked.

Cells adjacent to face zones that fall below the Proximity Threshold distance can also be tagged and

separated into new cell zones during the contact detection process. This is useful for specifying different

flow conditions in contact regions during the simulation.

To enable flow control options, select the Flow Control check box in the Contact Detection tab. Ad-

ditional settings for flow control can then be specified by clicking the Controls... button to display

the Flow Controls dialog box (see Figure . : The Flow Controls Dialog Box (p. )).

Figure . : The Flow Controls Dialog Box

In the Flow Controls dialog box, you can specify a flow control zone (for example, restrictions, and

so on) for any cell zone in the mesh. To create a flow control zone, select a zone from the Cell Zones

list, specify a new name in the Flow Control Zone text box, and click the Create Zone button. Once

the flow control zone has been created, it becomes available in the Cell Zone Conditions task page,

where additional physical properties (for example, inertial and/or viscous porous resistance) can be

specified. During the simulation, once cells in the contact region have been separated into new zones,

the physical properties specified in the respective flow control zone are copied to the newly separated

cell zone.

If you are simulating a transient flow, you can use the events in ANSYS Fluent to control the timing of

specific events during the course of the simulation. With in-cylinder flows for example, you may want

to open the exhaust valve (represented by a pair of deforming sliding interfaces) by creating an event

to create the sliding interfaces at some crank angle. You can also use dynamic mesh events to control

when to suspend the motion of a face or cell zone by creating the appropriate events based on the

crank angle or time. Note that in-cylinder flows are crank angle-based, whereas all other flows are

time-based.

.... Procedure for Defining Events

You can define the events using the Dynamic Mesh Events Dialog Box (p. ) (Figure . : The Dy-

namic Mesh Events Dialog Box (p. )).

Setup →

Figure . : The Dynamic Mesh Events Dialog Box

The procedure for defining events is as follows:

. Increase the Number of Events value to the number of events you want to specify. As this value is in-

creased, additional event entries in the dialog box will become editable.

. Enable the check box next to the first event and enter a name for the event under the Name heading.

. Specify either the time or the crank angle at which you want the event to occur.

For in-cylinder flows, specify the crank angle at which you want the event to occur under At Crank

Angle.

For non-in-cylinder flows, specify the time (in seconds) at which you want the event to occur under

At Time.

It is not necessary to specify the events in order of increasing time or crank angle, but it may be

easier to keep track of events if you specify them in the order of increasing time or angle.

. Click the Define... button to open the Define Event Dialog Box (p. ) (Figure . :The Define Event

Figure . : The Define Event Dialog Box

. In the Define Event Dialog Box (p. ), choose the type of event by selecting Change Zone Type, Copy

Zone BC, Activate Cell Zone, Deactivate Cell Zone, Create Sliding Interface, Delete Sliding Interface,

Change Motion Attribute, Change Time Step Size, Change Under-Relaxation Factors, Insert

Boundary Zone Layer, Remove Boundary Zone Layer, Insert Interior Zone Layer, Remove Interior

Zone Layer, Insert Cell Layer, Remove Cell Layer, Execute Command, Replace Mesh, Inert EGR Reset,

or Diesel Unsteady Flamelet Reset in the Type drop-down list.These event types and their definitions

are described later in this section.

. Repeat steps – for the other events, if relevant.

. Click Apply in the Dynamic Mesh Events Dialog Box (p. ) after you finish defining all events.

. To play the events to check that they are defined correctly, click the Preview... button in the Dynamic

Mesh Events Dialog Box (p. ).This displays the Events Preview Dialog Box (p. ).

For in-cylinder flows, you use the Events Preview Dialog Box (p. ) (Figure . : The Events

Preview Dialog Box for In-Cylinder Flows (p. )), to enter the crank angles at which you want to

start and end the playback in the Start Crank Angle and End Crank Angle fields, respectively.

For non-in-cylinder flows, you use the Events Preview Dialog Box (p. ) to enter the time at which

you want to start and end the playback in the Start Time and End Time fields, respectively.

Specify the size of the step to take during the playback in the Increment field. Click Preview to

play back the events. ANSYS Fluent will play the events at the time (or crank angle in the case of

in-cylinder flows) specified for each event and report when each event occurs in the text (console)

window.

Figure . : The Events Preview Dialog Box for In-Cylinder Flows

For in-cylinder simulations, you must specify the events for one complete engine cycle. In the

subsequent cycles, the events are executed whenever

(.)

where

is the event crank angle,

is the current crank angle calculated from   Equa-

tion . (p. ),

is the crank angle period for one cycle, and  is some integer.

As an example, for in-cylinder simulations, you are not required to specify the event crank angle

to correspond exactly to the current crank angle calculated from Equation . (p. ). ANSYS

Fluent will execute an event if the current crank angle is between

where

is the

equivalent change in crank angle for the time step. For example, if the event preview is executed

between crank angle of

and

(crank period is

) using an increment of

, ANSYS

Fluent will report the following in the text window.

Execute Event: open-in-valve-left (defined at: ., current angle: .)

Execute Event: open-in-valve-right (defined at: ., current angle: .)

Execute Event: close-ex-valve-right (defined at: ., current angle: .)

Execute Event: close-ex-valve-left (defined at: ., current angle: .)

Execute Event: close-in-valve-left (defined at: ., current angle: .)

Execute Event: close-in-valve-right (defined at: ., current angle: .)

Execute Event: open-ex-valve-right (defined at: ., current angle: .)

Execute Event: open-ex-valve-left (defined at: ., current angle: .)

Notice that events defined at

and

are executed at

and

, respectively, be-

cause they satisfy the condition of   Equation . (p. ).

.... Defining Events for In-Cylinder Applications

ANSYS Fluent will automatically limit the valve lift values depending on the specified minimum valve

lift value. However, the conversion of the sliding interface zones to walls (and vice versa) is accom-

plished via the in-cylinder events (see Defining Dynamic Mesh Events (p. )). For example, if the

exhaust valve closes at

before TDC position, you must define a Delete Sliding Interface event

at the crank angle of

. You must define similar events for the intake valve opening (using the

Create Sliding Interface event), the intake valve closing (Delete Sliding Interface event), and the

exhaust valve opening (Create Sliding Interface event) at the respective crank angles.

For the current example, the exhaust valve is assumed to be open between

and

and the

intake valve is open between at

and

.

..... Events

Each of the available events is described below.

..... Changing the Zone Type

You can change the type of a zone to be a wall, or an interface, interior, fluid, or solid zone during

your simulation. To change the type of a zone, select Change Zone Type in the Type drop-down

list in the Define Event Dialog Box (p. ) (Figure . : The Define Event Dialog Box (p. )). Select

the zone(s) that you want to change in the Zone list, and then select the new zone type in the New

Zone Type drop-down list.

..... Copying Zone Boundary Conditions

You can copy boundary conditions from one zone to other zones during your simulation. If, for ex-

ample, you have changed an inlet zone to type wall with the Change Zone Type event, you can

set the boundary conditions of the new zone type by simply copying the boundary conditions from

a known zone with the corresponding zone type.

To copy boundary conditions from one zone to another, select Copy Zone BC in the Type drop-

down list in the Define Event Dialog Box (p. ) (Figure . : The Define Event Dialog Box (p. )).

In the From Zone drop-down list, select the zone that has the conditions you want to copy. In the

To Zone(s) list, select the zone or zones to which you want to copy the conditions.

ANSYS Fluent will set all of the boundary conditions for the zones selected in the To Zone(s) list to

be the same as the conditions for the zone selected in the From Zone list. (You cannot copy a

subset of the conditions, such as only the thermal conditions.)

Note that you cannot copy conditions from external walls to internal (that is, two-sided) walls, or

vice versa, if the energy equation is being solved, since the thermal conditions for external and in-

ternal walls are different.

..... Activating a Cell Zone

To activate a cell zone, select Activate Cell Zone in the Type drop-down list in the Define Event

Dialog Box (p. ) (Figure . : The Define Event Dialog Box (p. )), then select the zone that you

want to activate in the Zone(s) list. For more information, see Replacing, Deleting, Deactivating, and

Activating Zones (p. ).

..... Deactivating a Cell Zone

To deactivate a cell zone, select Deactivate Cell Zone in the Type drop-down list in the Define Event

want to deactivate in the Zone(s) list.

Only deactivated zones can be activated. When a zone is deactivated, ANSYS Fluent skips the zone

during the calculations. For more information, see Replacing, Deleting, Deactivating, and Activating

..... Creating a Sliding Interface

To create a sliding interface during your simulation, select Create Sliding Interface in the Type

drop-down list in the Define Event Dialog Box (p. ) (Figure . : The Define Event Dialog Box for

the Creating Sliding Interface Option (p. )). Enter a name for the sliding interface in the Interface

Name field. Select the zones on either side of the interface in the Interface Zone  and Interface

Zone  drop-down lists.

You have the option to select any number of zones listed under each of the interface zones. ANSYS

Fluent calculates intersections between all possible combinations of the left and right side of the

interfaces, allowing you more flexibility in terms of creating zones and defining the interfaces.

Figure . : The Define Event Dialog Box for the Creating Sliding Interface Option

Important

If ANSYS Fluent finds another interface with the same name as defined in the event, then

the old interface will be deleted and a new one created as defined in the dynamic mesh

event.

If the interface zones that you selected above do not overlap each other completely, the non-over-

lapped regions on each interface zones are put into separate wall zones by ANSYS Fluent. If these

wall zones (that is, non-overlapped regions) have motion attributes associated with them, their

motion can only be specified by copying the motion from another dynamic zone by selecting the

appropriate dynamic zones in the Wall  Motion and Wall  Motion drop-down lists, respectively.

Note that you do not have to change the boundary type from wall to interface. When the Create

Sliding Interface event is executed, ANSYS Fluent will automatically change the boundary type of

the face zones selected in Interface Zone  and Interface Zone  to type interface before the sliding

interface is created.

..... Deleting a Sliding Interface

To delete a sliding interface that has been created earlier in your simulation, select Delete Sliding

Interface in the Type drop-down list in the Define Event Dialog Box (p. ) (Figure . : The Define

Event Dialog Box (p. )). Enter the name of the sliding interface to be deleted in the Interface

Name field.

As with the Create Sliding Interface event, ANSYS Fluent will automatically change the corresponding

interface zones to wall. However, you may want to use the Copy Zone BC event to set any boundary

conditions that are not the default conditions that ANSYS Fluent assumes.

..... Changing the Motion Attribute of a Dynamic Zone

To change the motion attribute of a dynamic zone during your in-cylinder calculation, select Change

Motion Attribute in the Type drop-down list in the Define Event Dialog Box (p. ) (Figure . : The

Define Event Dialog Box (p. )). Select the Attribute (smoothing or remeshing) and set the appro-

priate Status (enable or disable). Select the corresponding dynamic zones for which you want to

change the motion attributes in the Dynamic Zones list.

The smoothing attribute is used to enable or disable smoothing of nodes on selected deforming

face zones and the remeshing attribute is used to enable and disable face remeshing on selected

deforming face zones.

..... Changing the Time Step

To change the time step at some point during the simulation, select Change Time Step Size in the

Type drop-down list in the Define Event Dialog Box (p. ). Specify the new physical time step size

by entering the new Time Step Size in seconds.

For in-cylinder simulations, specify the new physical time step by entering the new Crank Angle

Step Size value in degrees. The physical time step is calculated from

(.)

..... Changing the Under-Relaxation Factor

To change one or more under-relaxation factors, select Change Under-Relaxation Factor in the

Type drop-down list in the Define Event Dialog Box (p. ) (Figure . : The Define Event Dialog

Box (p. )). Select the under-relaxation factor that you want to change, and assign a new value to

it in the Under-Relaxation Factors list. For more information on setting under-relaxation factors,

see Setting Under-Relaxation Factors (p. ).

..... Inserting a Boundary Zone Layer

To insert a new cell zone layer as a separate cell zone adjacent to a boundary, select Insert Boundary

Zone Layer in the Type drop-down list in the Define Event Dialog Box (p. ). Specify the Base

Dynamic Zone, from which the layer of cells is to be created, and the Side Dynamic Zone, which

represents the deforming face zone adjacent to the Base Dynamic Zone before the layer is inserted.

The new cell zone will inherit the boundary conditions of the cell zone adjacent to the Base Dynamic

Zone before the layer is inserted.

Note that a new cell layer can be inserted only from a one-sided Base Dynamic Zone. You cannot

insert a new cell layer from an interior face zone.

Figure . : Boundary Zone Before Insertion (p. ) and Figure . : Boundary Zone After Inser-

tion (p. ) illustrate the insertion of a boundary zone layer. In both figures, the circular face at the

top of the cylinder is the base dynamic zone.

Figure . : Boundary Zone Before Insertion

Figure . : Boundary Zone After Insertion

..... Removing a Boundary Zone Layer

To remove the cell zone layer inserted using the Insert Boundary Zone Layer event, select Remove

Boundary Zone Layer in the Type drop-down list in the Define Event Dialog Box (p. ). Specify

the same Base Dynamic Zone that you used when you defined the insert boundary layer event.

Note that a cell layer can be removed only from a one-sided Base Dynamic Zone.

..... Inserting an Interior Zone Layer

To insert a new zone layer as a separate cell zone adjacent to the internal side of a boundary, select

Insert Interior Zone Layer in the Type drop-down list in the Define Event Dialog Box (p. ). Specify

the Base Dynamic Zone and the Side Dynamic Zone as described in the Insert Boundary Zone

Layer event. You also must specify the names of the new interior face zones (Internal Zone  Name

and Internal Zone  Name) that will be created after the cell zone layer is created by ANSYS Fluent.

ANSYS Fluent inserts the interior cell layer by splitting the cell zone adjacent to the Base Dynamic

Zone with a plane. The position of the plane and the normal direction of the plane are implicitly

defined by the cylinder origin and cylinder axis of the Side Dynamic Zone.

Figure . : Interior Zone Before Insertion (p. ) and Figure . : Interior Zone After Insertion (p. )

illustrate the insertion of an interior zone layer.

Figure . : Interior Zone Before Insertion

Figure . : Interior Zone After Insertion

..... Removing an Interior Zone Layer

To remove the zone layer inserted using the Insert Interior Zone Layer event, select Remove In-

terior Zone Layer in the Type drop-down list in the Define Event Dialog Box (p. ). Specify the

same Internal Zone  Name and Internal Zone  Name that you used to define the Insert Interior

Zone Layer event.

..... Inserting a Cell Layer

To manually insert a new cell layer to the existing cell zone, select Insert Cell Layer in the Type

drop-down list in the Define Event Dialog Box (p. ). Specify the Adjacent Dynamic Face Zone

and the Direction Parameter. This can only work on zones that are suited for layering (see Applic-

ability of the Dynamic Layering Method (p. )).

..... Removing a Cell Layer

To manually remove a cell layer from an existing cell zone, select Remove Cell Layer in the Type

..... Executing a Command

To execute a command, select Execute Command in the Type drop-down list in the Define Event

Dialog Box (p. ) (Figure . : The Define Event Dialog Box (p. )). A command can be a series

of text or Scheme commands, or a macro you have defined (or will define) using the Define Macro

Dialog Box (p. ) (see Defining Macros (p. )). Enter the series of commands or the name of the

macro in the Command text-entry box.

Important

If the command to be executed involves saving a file, see Saving Files During the Calcu-

lation (p. ) for important information.

..... Replacing the Mesh

To replace the mesh and interpolate existing data onto the new mesh during your simulation, select

Replace Mesh from the Type drop-down list in the Define Event dialog box (Figure . : The

Define Event Dialog Box (p. )). Then, specify the replacement mesh under Mesh File. Enable In-

terpolate Data Across Zones if necessary (see Replacing the Mesh (p. ) for details).

..... Resetting Inert EGR

To convert burnt gases at the end of the cycle to inert for the next cycle, select Inert EGR Reset

from the Type drop-down list in the Define Event dialog box (Figure . : The Define Event Dialog

Box (p. )). Specify the Zone(s). For further details, see Resetting Inert EGR (p. ).

..... Diesel Unsteady Flamelet Reset

To simulate multiple-cycle internal combustion engines using diesel unsteady flamelets, select

Diesel Unsteady Flamelet Reset from the Type drop-down list in the Define Event dialog box

(Figure . : The Define Event Dialog Box (p. )). Specify the Zone(s). This event is only applicable

to and available with diesel unsteady flamelets with two or more flamelets. For further details, see

Resetting Diesel Unsteady Flamelets (p. ). Note that Diesel Unsteady Flamelet Reset is generally

preferable to Inert EGR Reset since an additional transport equation is avoided.

.... Exporting and Importing Events

If you want to save the events you have defined to a file, click Write... in the Dynamic Mesh Events

Dialog Box (p. ) and specify the Event File in The Select File Dialog Box (p. ).

To read the events back into ANSYS Fluent, click Read... in the Dynamic Mesh Events Dialog Box (p. )

and specify the Event File in The Select File Dialog Box (p. ).

You must define the motion of the dynamic zones in your model. If the zone is a rigid body, you can

use a profile or user-defined function (UDF) to define the motion of the rigid body or use the six DOF

solver. If the zone is a deforming zone, you can define the geometry and the parameters that control

the face or zone remeshing, if applicable. For a zone that is deforming and moving at the same time,

you can use a user-defined function to define the geometry and motion of the zone as they change

with time.

.... General Procedure

You will specify the motion of the dynamic zones in your model using the Dynamic Mesh Zones

dialog box

Setup →

Details about specifying different types of motion are provided in this section.

..... Creating a Dynamic Zone

When you have completed the specification of a dynamic zone, click Create in the Dynamic Mesh

Zones Dialog Box (p. ) to complete the specification and add the zone to the Dynamic Mesh

Zones list.

..... Modifying a Dynamic Zone

If you want to make a change to the specification of a dynamic zone, select the zone in the Dynamic

Mesh Zones list, change the specification, and then click Create in the Dynamic Mesh Zones Dialog

Box (p. ) to update the specification.

..... Checking the Center of Gravity

If a dynamic zone has solid body motion, you can view its current position and orientation of the

center of gravity (with respect to initial data) by selecting the zone in the Dynamic Mesh Zones list

and viewing the values under Center of Gravity Location and Rigid Body Orientation.

..... Deleting a Dynamic Zone

To delete a dynamic zone that you have specified, select the zone in the Dynamic Mesh Zones list,

and click Delete or Delete All. The zone or zones will be removed from the Dynamic Mesh Zones

list.

.... Stationary Zones

By default, if no motion (moving or deforming) attributes are assigned to a face or cell zone, then

the zone is not considered when updating the mesh to the next time step. However, there are cases

where an explicit declaration of a stationary zone is required. For example, if a cell zone is assigned

some solid body motion, the positions of all nodes belonging to the cell zone will be updated even

though some of the nodes may also be part of a non-moving boundary zone. An explicit declaration

of a stationary zone excludes the nodes on these zones when updating the node positions.

Figure . : The Dynamic Mesh Zones Dialog Box for a Stationary Zone

To define a stationary zone in your model, follow the steps below.

. Select the stationary zone in the Zone Names drop-down list.

. Select Stationary under Type.

. If the stationary zone is a face zone that is not a boundary of a CutCell dynamic cell zone, then define

the Cell Height in the Meshing Options tab for any Adjacent Zone that is involved in local remeshing

or dynamic layering.The Cell Height specifies the ideal height (

Equation . (p. ) of the adjacent cells. Make a selection in the Cell Height drop-down menu to

specify this value as either a constant or a compiled user-defined function.

If you select the constant option, enter a value in the Cell Height text-entry box.

If you choose to use a compiled user-defined function to define an ideal cell height that varies as

a function of time or crank angle, you must first define a DEFINE_DYNAMIC_ZONE_PROPERTY

UDF. After you have compiled the UDF source file, built a shared library, and loaded it into ANSYS

Fluent, the name of the UDF library will be available for selection in the Cell Height drop-down

list.

Refer to the Fluent Customization Manual for information about UDFs.

. If the stationary zone is a boundary of a CutCell dynamic cell zone (this is automatically detected if the

CutCell dynamic cell zone is created first), then enter values for the Maximum Mesh Size and Growth

Rate in the Meshing Options tab. If you have enabled Inflation Layers for the cell zone, then you will

also have the option to enable Zonal Inflation Layer Control on the boundary zone and specify local

inflation settings in the Inflation Settings dialog box (using the Settings... button). See Figure . :The

Dynamic Mesh Zones Dialog Box for a CutCell Boundary Zone (p. ) for an example of the Dynamic

Mesh Zones dialog box with the Meshing Options tab as it appears for CutCell boundary zones. (The

same meshing input is required at all CutCell boundary zones, whether the motion type is Stationary,

Rigid Body, Deforming, or User-Defined.)

Two different size functions are available to control the local mesh refinement:

soft size function

For this size function, the Cartesian mesh is locally refined such that the resulting mesh

size is smaller or equal to the Maximum Mesh Size specified.

mesh-based size function

size is locally of the same size as the input mesh provided.

The switch between using the soft or the mesh-based size function depends on the value entered

for the Maximum Mesh Size. A value of  specifies that the mesh-based size function is used. If

a positive value is entered, then the soft size-function is used and the value entered locally limits

the mesh size. The Growth Rate controls the rate at which the Cartesian mesh grows away from

the boundary. The maximum Cartesian mesh size obtained in the cell zone is always controlled

by the specified Maximum Mesh Size for the CutCell cell zone.

Figure . : The Dynamic Mesh Zones Dialog Box for a CutCell Boundary Zone

You can view the vital statistics of your zone by clicking on the Zone Scale Info… button. This

opens the Zone Scale Info Dialog Box (p. ), where you can view the minimum, maximum, and

average length scale values, as well as the maximum skewness value.

. For cases with strong fluid-structure interaction, solution stabilization may help convergence for

boundary zones. Solution stabilization can be set in the Solver Options tab. See Solution Stabilization

for Dynamic Mesh Boundary Zones (p. ) for details.

Note that if you specify inflation layer parameters in the Inflation Settings dialog box, these

settings are not saved until you create or update the dynamic zone.

.... Rigid Body Motion

To define a rigid-body zone in your model, follow the steps below.

Figure . : The Dynamic Mesh Zones Dialog Box for a Rigid Body Motion

. Select the rigid body zone in the Zone Names drop-down list.

. Select the Rigid Body option under Type.

. If you want to specify the motion of the rigid body zone using a profile or user-defined function, then

select a profile or user-defined function from the Motion UDF/Profile drop-down list in the Motion

Attributes tab. See Profiles (p. ) and Solid-Body Kinematics (p. ) for information on profiles, and

see the Fluent Customization Manual for information on user-defined functions.

. If you enabled the In-Cylinder option in the Dynamic Mesh Task Page (p. ), ANSYS Fluent provides

built-in functions in the Motion UDF/Profile drop-down list that can be useful for defining the rigid

body motion of a piston. If you would like the motion of the piston to be a function of crank angle (that

is, governed by Equation . (p. )), then you should select **piston-full**. For further information,

see In-Cylinder Settings (p. ).

. If you enabled the Six DOF option in the Dynamic Mesh Task Page (p. ), make sure that On is enabled

in the Six DOF group box in the Motion Attributes tab (see Figure . :The Dynamic Mesh Zones

Dialog Box for a Rigid Body Motion Using the Six DOF Solver (p. )), to ensure that the six DOF solver

is being used.Then make a selection from the Six DOF UDF/Properties drop-down list; for details on

creating the selections available in this list, Setting Rigid Body Motion Attributes for the Six DOF Solv-

er (p. ).

Note that the Passive option in the Six DOF group box is used when you do not want the forces

and moments on the zone to be taken into consideration.

. Specify the initial location of the center of gravity for the rigid body by entering coordinates in

the Center of Gravity Location group box.

. If you want a rigid body to move relative to another rigid body, then you must enable Relative Motion

and specify the Relative Zone.

Note

You must create the relative rigid body zone before creating a rigid body that is de-

pendent on that zone, if you are setting up the motion using the graphical user interface

(GUI). The order in which you specify the zones does not matter if you set up the motion

using the text user interface (TUI).

. Specify the orientation of the rigid body (in the inertial coordinate system) by entering the orientations

of the rigid body in Rigid Body Orientation.

Together, the Rigid Body Orientation and the Center of Gravity Location are the local reference

frame that you can choose to use for your user-defined function (UDF) or set of six DOF properties that

describes the motion of the rigid body. For additional information about creating UDFs for solid-body

kinematics, see DEFINE_CG_MOTION in the Fluent Customization Manual; for details on creating

UDFs / properties for the six DOF solver, see Setting Rigid Body Motion Attributes for the Six DOF

Solver (p. ).

For most cases, this is an initial reference orientation that ANSYS Fluent later updates, letting you

keep track of the object’s current orientation. The rigid body orientation is most useful when using

the six DOF solver, where it is used to compute the transformation matrices (Six DOF Solver Theory

in the Theory Guide).

If needed, you can use the Orientation Calculator to convert a rotation matrix or Euler angles

into the required axis and angle inputs. You can also use this calculator if you know the rotations

the rigid body will experience, but do not know its final orientation.

Figure . : Orientation Calculator Dialog Box

To use the Orientation Calculator:

a.

Enter a value, either in Axis and Angle, Rotation Matrix, or Euler Angle format, and click Evaluate

to see the value in the output format.

The calculator also converts the entered values into the other two “grayed-out” input formats.

Note

There are several possible Euler angle representations. Fluent uses a vector defined

by

,

, and

where:

Note

by

,

, and

where:

is the rotation about the original Z axis,

is the rotation

about the rotated Y axis, and

is the rotation about the rotated X axis.

b. Enable Concatenate Next Input if you want the next input to be concatenated to the previous output.

c.

Click Fill to use the current Output as your Rigid Body Orientation in the Dynamic Mesh Zones

. When using the six DOF solver, specify the velocity of the center of gravity with respect to the inertia

coordinate system by entering the velocity of the center of gravity in Center of Gravity Velocity. Also,

specify the angular velocity of the rigid body with respect to the inertia coordinate system by entering

the angular velocity of the rigid body in Rigid Body Angular Velocity. Note that these fields are ignored

for one DOF rotation and translation, respectively.

Figure . : The Dynamic Mesh Zones Dialog Box for a Rigid Body Motion Using the Six

DOF Solver

. If you are solving an in-cylinder problem, specify the direction of the reference axis of the valves or piston

in Valve/Piston Axis.

The current valve lift or piston stroke is automatically updated in Lift/Stroke when you click

Create based on the parameters you have specified earlier when you first invoke the in-cylinder

option.

. By default, the boundary mesh motion is taken into consideration when imposing the physical boundary

conditions, even if the boundary moves because of a moving adjacent cell zone and no dynamic zone

has been created for the boundary. If this is not the desired behavior, and if you would like to exclude

the mesh motion from contributing to the boundary conditions, then you need to enable the Exclude

Mesh Motion in Boundary Conditions option for that zone.

. If the rigid body zone is a face zone that is not a boundary of a CutCell dynamic cell zone, specify the

Cell Height for each Adjacent Zone in the Meshing Options tab.The Cell Height is the ideal cell height

(

in Equation . (p. ) and Equation . (p. ) that is used by ANSYS Fluent to determine

when the prismatic layer next to the rigid body should be split or merged with the layer next to it. If the

adjacent zone is tetrahedral or triangular, the ideal height is used by ANSYS Fluent to determine if adjacent

cells must be agglomerated for local remeshing. Make a selection in the Cell Height drop-down menu

to specify this value as either a constant or a compiled user-defined function.

list.

. If the rigid body zone is a boundary of a CutCell dynamic cell zone (this is automatically detected if the

Rate in the Meshing Options tab, as described in step  of Stationary Zones (p. ). If you have enabled

Inflation Layers for the cell zone, then you will also have the option to enable Zonal Inflation Layer

Control on the boundary zone and specify local inflation settings in the Inflation Settings dialog box

(using the Settings... button).

. If the dynamic zone is a face zone with an adjacent boundary layer mesh, you must apply boundary

layer smoothing using the Deform Adjacent Boundary Layer with Zone option in the Meshing Options

tab if you want the boundary layer to move with the moving face zone. For example, this option is ne-

cessary if you are applying face region remeshing with prism layers and you have not decomposed the

mesh volume (see Face Region Remeshing with Wedge Cells in Prism Layers (p. )). In such circumstances,

the Deform Adjacent Boundary Layer with Zone option ensures that the base prism elements shown

in Figure . :Volume Decomposition for the Base of the Prism Layers (p. ) will move rigidly with

the piston.

Note that the boundary layer smoothing method is primarily intended for translational motion of

the face zone. If significant rotation is applied to the face zone, the boundary layer cells may be-

come skewed. For more information refer to Boundary Layer Smoothing Method (p. ).

. For cases with strong fluid-structure interaction, solution stabilization may be necessary for boundary

zones if the use of implicit mesh updating (described in Implicit Update Settings (p. )) is insufficient

to stabilize the solver due to the fluid motion. Solution stabilization options can be set in the Solver

Options tab. See Solution Stabilization for Dynamic Mesh Boundary Zones (p. ) for details.

.... Deforming Motion

To define a deforming zone in your model, follow the steps below.

Figure . : The Dynamic Mesh Zones Dialog Box for a Deforming Motion with Cell Zone

Options

. Select the deforming zone in the Zone Names drop-down list.

. Select the Deforming option under Type.

. Specify the geometry of the deforming zone in the Geometry Definition tab.

If no geometry is available, select faceted in the Definition drop-down list.

If the geometry is a plane, select plane in the Definition drop-down list.To define the plane, enter

the position of a point on the plane in Point on Plane and the plane normal in Plane Normal.

If the geometry is a cylinder, select cylinder in the Definition drop-down list.To define the cylinder,

enter the Cylinder Radius, the Cylinder Origin and the Cylinder Axis.

If the geometry is unspecified and mesh motion normal to the boundary is permissible, select unspe-

cified in the Definition drop-down list.This option is only available if the linearly elastic solid mesh

smoothing method is enabled (Linearly Elastic Solid Based Smoothing Method (p. )).

If the geometry is described by a user-defined function, select user-defined in the Definition drop-

down list and the appropriate user-defined functions in the Geometry UDF drop-down list. See the

Fluent Customization Manual for information on user-defined functions.

For 3D simulations, ANSYS Fluent allows you to preserve features on the boundary zones that are

important for the flow. Such features may be at the juncture of different boundary zones, or they

may be on a single non-planar boundary zone. For any geometry definition (faceted, plane, cyl-

inder, or user-defined), you can indicate whether you want to preserve features of a specific

angular range by enabling Feature Detection under Feature Options and setting a threshold

value for the Feature Angle in degrees. For more information (including how the Feature Angle

is defined), see Feature Detection (p. ).

When available, the geometry information is used to project nodes on the deforming zone after

remeshing the face zone, or if nodes are moved through smoothing.

. For deforming boundary and cell zones that are not CutCell zones, specify the appropriate

remeshing parameters in the Meshing Options tab.

You can locally enable Remeshing and define the settings in the group box under this option, including

Under Parameters, enabling the Global Settings option ensures that settings defined in the

Mesh Method Settings Dialog Box (p. ) are used for this dynamic zone. Disabling this option

allows you to revise the Minimum Length Scale, Maximum Length Scale and/or Maximum

Skewness locally. When setting these values, you should use the vital statistics of your zone

found in the Zone Scale Info Dialog Box (p. ), which can be opened by clicking the Zone

Scale Info... button.

For boundary zones, under Options you can specify the remeshing methods applied to this

dynamic zone, including Region and Local.

You can locally enable Smoothing and, if Spring/Laplace/Boundary Layer is selected for smoothing

in the Mesh Method Settings Dialog Box (p. ), define the settings in the group box under this option,

including the following:

If you selected a cell zone, enabling the Global Settings option ensures that the element type

defined in the Mesh Smoothing Parameters Dialog Box (p. ) is used for this dynamic zone.

Disabling it allows you to select a different element type locally.

If you selected a boundary zone, you can specify whether the smoothing method is spring

based or Laplacian.

. To specify that a deforming cell zone is remeshed using the CutCell zone method, ensure that

Remeshing is enabled in the Meshing Options tab, and enable the CutCell option under Options

(see Figure . : The Dynamic Mesh Zones Dialog Box for a Deforming CutCell Cell Zone (p. )).

Note that this option is only available if you have previously enabled the CutCell Zone option in

the Remeshing tab of the Mesh Method Settings dialog box (see Figure . : The Remeshing

Tab in the Mesh Method Settings Dialog Box (p. )).

Figure . : The Dynamic Mesh Zones Dialog Box for a Deforming CutCell Cell Zone

After the CutCell option has been enabled, you must enter values for the global CutCell parameters

Maximum Mesh Size and Growth Rate, as well as the controls for the remeshing frequency,

Minimum Orthogonal Quality and Remeshing Interval. You also have the option to enable In-

flation Layers for the cell zone and specify the global inflation parameters in the Inflation Settings

dialog box. See Using the CutCell Zone Remeshing Method (p. ) for more information about

adding inflation layers to a CutCell mesh.

The Maximum Mesh Size specified for the CutCell cell zone controls the global maximum size

of the Cartesian cells. The global Growth Rate is used for all mesh-based size functions applied

to CutCell boundary zones that are not defined as dynamic zones. When selecting values for these

controls, it may be helpful to view the statistics of your cell zone by clicking on the Zone Scale

Info... button. This opens the Zone Scale Info Dialog Box (p. ), where you can view the minimum

and maximum length scale values, as well as the maximum skewness values.

The CutCell remeshing is performed automatically whenever cells exhibit an orthogonal quality

(as defined in Mesh Quality (p. )) that is less than the specified Minimum Orthogonal Quality.

The remeshing is also performed periodically after the calculation has undergone the number of

time steps you specified for the Remeshing Interval.

Click the Boundary Zones Info... button to open the CutCell Boundary Zones Info dialog box

(Figure . : The CutCell Boundary Zones Info Dialog Box (p. )). This dialog box lists all the

boundary zones associated with the CutCell cell zone, along with the associated size functions

and zonal meshing parameters. The inflation layer settings used on all boundaries are also shown.

It is recommended that you revisit this dialog box after you have created all of the dynamic zones,

in order to review all of the parameters you have set.

Figure . : The CutCell Boundary Zones Info Dialog Box

You can also enable local Smoothing and revise the associated settings, as described previously

for deforming zones that are not CutCell zones.

. If the deforming zone is a boundary of a CutCell dynamic cell zone (this is automatically detected if the

Rate in the Meshing Options tab, as described in step . of Stationary Zones (p. ). If you have enabled

.... User-Defined Motion

For a zone that is deforming and/or moving, you can define the position of each node on the general

deforming / moving zone using a user-defined function (UDF). To define a moving / deforming zone,

follow the steps below.

. Select the moving and deforming zone in the Zone Names drop-down list.

. Select the User-Defined option under Type.

. In the Motion Attributes tab, select the user-defined function that defines the geometry and motion

of the zone from the Mesh Motion UDF drop-down list. See the Fluent Customization Manual for inform-

ation on user-defined functions used to specify user-defined motion.

. By default, the boundary mesh motion is taken into consideration when imposing the physical

boundary conditions. If this behavior is not desired and you would instead like to exclude the

mesh motion from contributing to the boundary conditions, then you need to enable the Exclude

Mesh Motion in Boundary Conditions option for that boundary zone. The following are examples

of when you might want to exclude such motion:

You have created a dynamic zone for a cell zone that moves, but one or more of the boundaries of

that cell zone should be treated as stationary.

You are using a DEFINE_GRID_MOTION UDF that defines nodal motion on a boundary that, for ex-

ample, includes both rigid body motion (which should contribute to the boundary condition) and

smoothing (which should not).With such UDFs, you must perform the following steps for that

boundary:

– Enable the Exclude Mesh Motion in Boundary Conditions option.

– Define the rigid body motion in the Momentum tab of the Wall dialog box.

. If you want the movement / deformation to be relative to the rigid body motion of a cell zone, then you

can enable Relative Motion and select the cell zone from the Relative Zone list.

Note

You must specify the movement / deformation in your UDF using NODE_COORD_NEST,

rather than specify the final coordinates (as you would if you were NOT specifying it

relative to a cell zone). For additional information, see DEFINE_GRID_MOTION in the

You must create the relative rigid body zone before creating the user-defined zone if

you are setting up the zones using the graphical user interface (GUI). The order in which

you create the zones does not matter if you set up the zones using the text user inter-

face (TUI).

. For a face zone that is not a boundary of a CutCell dynamic cell zone, you can specify the Cell Height in

the Meshing Options tab for any Adjacent Zone that is involved in local remeshing or dynamic layering.

The Cell Height specifies the ideal height (

in Equation . (p. ) and Equation . (p. ) of

the adjacent cells. Make a selection in the Cell Height drop-down menu to specify this value as either a

constant or a compiled user-defined function.

list.

Refer to the separate Fluent Customization Manual for information about UDFs.

. If the face zone is a boundary of a CutCell dynamic cell zone (this is automatically detected if the CutCell

dynamic cell zone is created first), then enter values for the Maximum Mesh Size and Growth Rate in

the Meshing Options tab, as described in step  of Stationary Zones (p. ). If you have enabled Inflation

Layers for the cell zone, then you will also have the option to enable Zonal Inflation Layer Control on

the boundary zone and specify local inflation settings in the Inflation Settings dialog box (using the

Settings... button).

. If the dynamic zone is a face zone with an adjacent boundary layer mesh, and you want to use the

boundary layer smoothing method (as described in Boundary Layer Smoothing Method (p. )), enable

the Deform Adjacent Boundary Layer with Zone option in the Meshing Options tab.

. For a 3D boundary zone, you can allow local face remeshing by enabling the Local option (under

Remeshing Methods) in the Meshing Options tab. For details, see Local Face Remeshing Method (p. ).

Enabling this option allows you to do the following:

You can revise the Maximum Skewness allowed for faces if you want to specify a local value for this

dynamic zone that differs from the one you specified globally in the Mesh Method Settings Dialog

Box (p. ). Note that the global setting may still be used if ANSYS Fluent determines that your local

setting is unreasonable.

You can preserve features, not only at the juncture of different boundary zones, but also on a single

non-planar boundary zone. In the Geometry Definition tab, you can indicate whether you want to

include features of a specific angular range by enabling Feature Detection under Feature Options

and setting a threshold value for the Feature Angle in degrees. For more information (including how

the Feature Angle is defined), see Feature Detection (p. ).

. If this zone is part of a mesh interface and only one side undergoes user-defined motion, then by default

that motion will be transferred to the other side in order to maintain the coupling.You can change the

method by which the displacement of the passive nodes is calculated or disable this transfer altogether,

as described in Transferring Motion Across a Mesh Interface (p. ).

..... Specifying Boundary Layer Deformation Smoothing

For a boundary layer that deforms according to the adjacent face zone, the zone that is deforming

and moving is usually defined using a user-defined function (UDF), as described in User-Defined

Motion (p. ). To define a moving and deforming boundary layer, perform the steps that follow.

If the boundary layer borders a face zone that is only moving and is not deforming, you should

consider applying rigid body motion to the face zone (see Rigid Body Motion (p. )) rather than

user-defined motion, as rigid body motion usually involves a simpler UDF.

.

Set up the moving and deforming zone.

a.

Select the moving and deforming zone in the Zone Names drop-down list.

b.

Select User-Defined from the Type list.

c.

In the Motion Attributes tab, select the user-defined function that defines the geometry and

b.

c.

motion of the zone from the Mesh Motion UDF drop-down list.

d.

In the Meshing Options tab, enable the Deform Adjacent Boundary Layer with Zone option.

e.

.

Set up a deforming dynamic zone for the fluid zone that contains the boundary layer.

a.

Select the fluid zone that contains the boundary layer from the Zone Names drop-down list.

b.

Select Deforming from the Type list.

c.

In the Meshing Options tab, ensure that Remeshing and Smoothing are enabled.

d.

.

If the fluid zone set up in the step  consists entirely of the boundary layer elements, set up a deforming

dynamic zone for the neighboring fluid zone.This step is necessary because the deforming boundary

layer will deform the adjacent cells.

a.

Select the fluid zone that neighbors the boundary layer zone from the Zone Names drop-down

list.

b.

Select Deforming from Type list.

c.

In the Meshing Options tab, enable Smoothing and Remeshing in the Methods group box.

d.

.... System Coupling Motion

For a zone that is involved in a system coupling, the motion is defined by the application that ANSYS

Fluent is coupled with on this zone. For more details about setting up a simulation with system

coupling see Performing System Coupling Simulations Using Fluent (p. ) and the System Coupling

User's Guide. To define a system coupling region, follow the steps below.

. Select the System Coupling option under Type.

. The system coupling region cannot be a boundary of a CutCell dynamic cell zone, so you can specify the

Cell Height in the Meshing Options tab for any Adjacent Zone that is involved in local remeshing or

dynamic layering.The Cell Height specifies the ideal height (

in Equation . (p. ) and Equa-

tion . (p. ) of the adjacent cells. Make a selection in the Cell Height drop-down menu to specify

this value as either a constant or a compiled user-defined function.

list.

. For cases with strong fluid-structure interaction, solution stabilization may be necessary to achieve

convergence for boundary zones undergoing system coupling motion. Solution stabilization options

can be set in the Solver Options tab. See Solution Stabilization for Dynamic Mesh Boundary Zones (p. )

. If this zone is part of a mesh interface and only one side undergoes system coupling motion, then by

default that motion will be transferred to the other side in order to maintain the coupling.You can change

the method by which the displacement of the passive nodes is calculated or disable this transfer alto-

gether, as described in Transferring Motion Across a Mesh Interface (p. ).

Note

If the System Coupling option is enabled, and ANSYS Fluent is not involved with a system

coupling simulation, then this zone type behaves in the same way as a stationary zone.

.... Intrinsic FSI Motion

For a two-way intrinsic fluid-structure interaction (FSI) simulation, you can specify that a wall zone

between a fluid and solid cell zone deforms according to the deformation of the adjacent solid zone

by performing the following steps. For more details about setting up an intrinsic FSI simulation, see

Setting Up an Intrinsic Fluid-Structure Interaction (FSI) Simulation (p. ).

Figure . : The Dynamic Mesh Zones Dialog Box for an Intrinsic FSI Zone

. Select a wall zone that is between a fluid and solid cell zone in the Zone Names drop-down list. Note

that this zone must be the side of a two-sided wall (that is, the wall or wall-shadow) that is immediately

adjacent to the fluid cell zone (as indicated by the Adjacent Cell Zone field in the Wall dialog box).

. Select Intrinsic FSI from the Type list. Note that this type is only available when you have selected a

model in the Structural Model Dialog Box (p. ).

list.

.... Solution Stabilization for Dynamic Mesh Boundary Zones

For cases with strong fluid-structure interaction, stabilization is achieved through a boundary source

coefficient introduced in the continuity equation, designed to improve the diagonal dominance of

the matrix system in the cells adjacent to dynamic mesh boundary zones. Two methods for this

boundary source coefficient are available:

volume-based

This method uses the cell volume

to re-scale the diagonal entry of the linear matrix system

corresponding to the discretized continuity equation (

) as

:

(.)

coefficient-based

This method directly re-scales the diagonal entry of the linear matrix system corresponding

to the discretized continuity equation (

) as

:

(.)

where

is the scale factor and  is the number of cells. Note that the value you choose for

will

only affect the rate of convergence, and will not affect the converged solution.

Note

While solution stabilization is available for all types of dynamic mesh boundary zones, it

is more commonly needed for rigid body motion with the six degrees of freedom (six DOF)

solver or for system coupling motion. It is not recommended for boundary zones of type

interior, as it can adversely affect convergence.

Solution stabilization can be enabled for a boundary zone by opening the Solver Options tab in the

Dynamic Mesh Zones Dialog Box (p. ), enabling the Solution Stabilization option, and then defining

the settings under Stabilization Parameters. Available settings include the Scale Factor (

) and the

Method, which can be either volume-based or coefficient-based (default). The Scale Factor must

be set to a nonzero value for the stabilization to have an effect.

The solver option settings can also be defined using the define/dynamic-mesh/zones/create

text command, and a summary of these settings can be printed in the console for each dynamic zone

by using the define/dynamic-mesh/zones/list text command.

.... Solid-Body Kinematics

ANSYS Fluent uses solid-body kinematics if the motion is prescribed based on the position and orient-

ation of the center of gravity of a moving object. This is applicable to both cell and face zones.

The motion of the solid-body can be specified either as a profile or as a user-defined function (UDF).

A profile may be defined by the following profile fields:

time (time)

crank angle (angle) (in-cylinder flows only)

position ( ,

, )

linear velocity (

,

,

)

angular velocity (

,

,

)

orientation (

,

,

)

For in-cylinder simulations, the velocity profiles for valves can be expressed as a function of crank

angle instead of time. In addition, transient boundary condition profiles can also be expressed as a

function of crank angle instead of time. For more information about transient profiles, see Defining

Transient Cell Zone and Boundary Conditions (p. ).

Below are two examples of a profile format:

((movement_linear  point)

(time

)

(x

)

(v_y

)

)

(time

)

(x

)

(v_y

)

)

((movement_angular  point)

(time

)

(omega_x

)

)

For in-cylinder flows, crank angles can be included in transient tables as well as transient profiles, in

a similar fashion to time. An example of a transient table using (crank) angle is as follows:

example

An example of a transient profile using (crank) angle is as follows:

(angle

)

In addition to the motion description, you must also specify the starting location of the center of

gravity and orientation of the solid body. In 2D cases (and 3D cases that do not use the six DOF

solver), ANSYS Fluent automatically updates the center of gravity position and orientation at every

time step such that

(.)

where

and

are the position and orientation of the center of gravity,

and

are the linear

and angular velocities of the center of gravity. 3D, six DOF cases use a more complex form of Equa-

tion . (p. ) when updating .

Typically,

is chosen to be an appropriate set of Euler angles. In this case, the solid-body motion

must be specified using a user-defined function (DEFINE_CG_MOTION).

Figure . : Solid Body Rotation Coordinates

The position vectors on the solid body are updated based on rotation about the instantaneous angular

velocity vector

. For a finite rotation angle

=

, the final position of a vector

on the

solid body with respect to

can be expressed as (See Figure . : Solid Body Rotation Coordin-

ates (p. ))

(.)

where

(.)

=

on the

ates (p. ))

(.)

where

(.)

The unit vectors

and

are defined as

(.)

(.)

If the solid body is also translating with

, the

position vector on the solid body can be expressed

as

(.)

where

is given by Equation . (p. ).

When you have specified the mesh update methods and their associated parameters, and you have

defined the motion of dynamic zones, as described in Specifying the Motion of Dynamic Zones (p. ),

you can preview the motion of the mesh or the zone as it changes with time before you start your

simulation. The same dynamic zone or mesh motion will be executed when you start your simulation.

.... Previewing Zone Motion

You can preview the motion of zones with Rigid Body or User-Defined motion using the Zone Motion

Dialog Box (p. ) (Figure . : The Zone Motion Dialog Box (p. )).

Setup →

Figure . : The Zone Motion Dialog Box

The zone motion preview only updates the graphical representation (in the graphics window) of the

zones that you have selected in the Dynamic Face Zones list. Only zones that have been specified

with either User-Defined or Rigid Body motion type are available for zone motion preview. To use

the Zone Motion preview:

. In the Zone Motion Dialog Box (p. ), select the face zones for which you want to preview the motion

from the Dynamic Face Zones list.The Dynamic Face Zones list displays zones that have either User-

Defined or Rigid Body motion specified. By default, all such zones are selected.

. Enter the Start Time, Time Step, and Number of Steps under Time Control.

. Click the Preview button to preview the zone motion.This positions the mesh according to the specified

Start Time, and then integrates the position of the selected surfaces in time.The zone positions at the

specified Start Time can be previewed without any subsequent motion by entering  for the Number

of Steps.

. Click Reset to restore the mesh to its initial state.

Previewing the zone motion can also be used as a postprocessor for six DOF simulations (see Six DOF

Solver Settings (p. )).

.... Previewing Mesh Motion

The mesh motion preview is different from the zone motion described above in that the mesh con-

nectivity is changed in mesh motion.

To preview the dynamic mesh of a transient case, you can use the Mesh Motion Dialog Box (p. )

(Figure . : The Mesh Motion Dialog Box (p. ))

Setup →

Figure . : The Mesh Motion Dialog Box

. Save the case file.

Important

Note that the mesh motion will actually update the node locations as well as the con-

nectivity of the mesh, so you must be sure to save your case file before doing the dy-

namic mesh motion. Once you have advanced the mesh by a certain number of time

steps, you will not be able to recover the previous status of the mesh, other than by

reloading the appropriate ANSYS Fluent case file.

. Specify the Number of Time Steps and the size of each time step (Time Step Size).The current time

will be displayed in the Current Mesh Time field after the dynamic mesh has been advanced the specified

number of steps.

Note that if you turned on the in-cylinder option, the Time Step Size is automatically calculated

from the Crank Angle Step Size and the Crank Shaft Speed that you have specified in the In-

Cylinder tab of the Options Dialog Box (p. ).

. To view the dynamic mesh in the graphics window, enable the Display Mesh option. In addition, you

can control the frequency at which ANSYS Fluent should display an updated mesh in the Display Fre-

quency field.To save a picture file of the mesh each time ANSYS Fluent updates it during the preview,

turn on the Save Picture option.This opens the Save Picture Dialog Box (p. ) (see Saving Picture

. Turn on Enable Autosave to use the automatic saving feature to specify the file name and frequency

with which case and data files should be saved during the solution process.This opens the Autosave

Case During Mesh Motion Preview Dialog Box (p. ).

. Enable the Update Mesh Interfaces option to update the interface at every time step.

. Enable the Update Overset Interfaces option to update the overset interface at every time step.

. Use the Update Monitors option to disable the processing of monitors and computation activities during

mesh motion preview.This allows you to set up monitors and computational activities before running

mesh motion preview without creating monitor files during the mesh motion preview.

. Click Preview to start the preview. ANSYS Fluent will update the dynamic mesh by moving and deforming

the face and cell zones that you have specified as dynamic zones. Click Apply to save your settings for

mesh motion.

During the preview, information about the dynamic mesh will be displayed in the console window

for each time step. Note that for the in-cylinder option, the reported Maximum Cell Skew is cal-

culated only from zones undergoing remeshing. This ensures that you can always ascertain whether

the skewness is increasing in the deforming zones. To report the maximum skewness of a cell from

any zone, you can click the Report Quality button in the General Task Page (p. ).

Setup →

While many dynamic mesh problems are transient, you can use dynamic meshes for steady-state ap-

plications as well. Some examples of steady-state applications include: checking the valve application

after reaching a steady-state valve position; or after a fluid-structure interface application has reached

a steady-state solution.

There are no differences in the meshing aspect between steady-state cases and transient cases. Fur-

thermore, setting up a steady-state simulation is similar to setting up a transient case, described in

Using Dynamic Meshes (p. ). However, there are a few differences that you should note:

A CG_MOTION UDF is needed to specify the motion of the boundary: a transient profile used in transient

cases cannot be used in steady-state cases.

The dtime passed to the CG_MOTION UDF is  by default: if a displacement of  mm is needed to move

the boundary, you can specify the velocity to be 1e- m/s.

Dynamic mesh parameters can be different since an interpolation error is no longer a concern.

If you have enabled local remeshing for your steady-state application, you can instruct ANSYS Fluent to

perform additional remeshing after the boundary has moved.This additional remeshing is based on

skewness criteria, and can further increase the quality of your mesh. See Dynamic Mesh Update Meth-

ods (p. ) for further details.

The mesh must be manually updated through journal files or execute commands. To update the mesh,

you can use the Mesh Motion Dialog Box (p. ).

Solution →

Run Calculation → Update Dynamic Mesh...

Alternatively, you can use the following text command:

solve → mesh-motion

which can also be used as an execute command in the Execute Commands Dialog Box (p. ):

Note

When you are solving a problem using the six DOF solver, you may need to modify the

pseudo time step size in order for the solver to converge. It is also recommended that you

ensure that the steady-state solution is reasonably well converged before performing the

steady-state dynamic mesh update.

Solution → Calculation Activities → Execute Commands

New...

You can display dynamic mesh statistics (such as minimum and maximum volumes and maximum cell

and face skewness) by clicking the Update button in the Mesh Motion Dialog Box (p. ) (Fig-

ure . : The Mesh Motion Dialog Box for Steady-State Dynamic Meshes (p. )).

Figure . : The Mesh Motion Dialog Box for Steady-State Dynamic Meshes

Important

The following options are not available for steady-state applications:

In-Cylinder

Implicit Update

Also, the Dynamic Mesh Events dialog box is not available for steady-state applications.

.... An Example of Steady-State Dynamic Mesh Usage

Consider a rescue drop case shown in Figure . : Initial Object Position (p. ). The object can be

moved in any position in the steady-state solver, after which steady-state analyses can be performed

at different object positions.

Figure . : Initial Object Position

The dynamic mesh parameters setup is identical for the steady-state and transient cases, which is

described in Setting Dynamic Mesh Modeling Parameters (p. ). When setting up the dynamic zones,

the procedures are similar to those described in Specifying the Motion of Dynamic Zones (p. ),

except that the UDF selected from the Motion UDF/Profile drop-down list is different. In steady-state

cases the dtime passed to the UDF is by default . So, in this example, the object will move  mm

each time the following UDF is executed:

DEFINE_CG_MOTION(pod,dt,vel,omega,time,dtime)

{

NV_S(vel,=,);

NV_S(omega,=,);

vel[] = -50e-;

}

The resulting mesh is shown in Figure . : Final Object Position After  Executions (p. ).

Figure . : The Mesh Motion Dialog Box After  Updates

Figure . : Final Object Position After  Executions

Chapter : Modeling Turbulence

This chapter provides details about how to use the turbulence models available in ANSYS Fluent.

Information about turbulence modeling theory is presented in Turbulence in the Theory Guide. Inform-

ation about using the turbulence models can be found in the following sections:

.. Choosing a Turbulence Model

.. Steps in Using a Turbulence Model

.. Setting Up the Spalart-Allmaras Model

.. Setting Up the k-ε Model

.. Setting Up the k-ω Model

.. Setting Up the Transition k-kl-ω Model

.. Setting Up the Transition SST Model

.. Setting Up the Intermittency Transition Model

.. Setting Up the Reynolds Stress Model

.. Setting Up Scale-Adaptive Simulation (SAS) Modeling

.. Setting Up the Detached Eddy Simulation Model

.. Setting Up the Large Eddy Simulation Model

.. Model Constants

.. Setting Up the Embedded Large Eddy Simulation (ELES) Model

.. Setup Options for All Turbulence Modeling

.. Defining Turbulence Boundary Conditions

.. Providing an Initial Guess for k and ε (or k and ω)

.. Solution Strategies for Turbulent Flow Simulations

.. Postprocessing for Turbulent Flows

Turbulence is the three-dimensional unsteady random motion observed in fluids at moderate to high

Reynolds numbers. As technical flows are typically based on fluids of low viscosity, almost all technical

flows are turbulent. Many quantities of technical interest depend on turbulence, including:

Mixing of momentum, energy and species

Heat transfer

Pressure losses and efficiency

Forces on aerodynamic bodies

While turbulence is, in principle, described by the Navier-Stokes equations, it is not feasible in most

situations to resolve the wide range of scales in time and space by Direct Numerical Simulation (DNS)

as the CPU requirements would by far exceed the available computing power for any foreseeable future.

For this reason, averaging procedures have to be applied to the Navier-Stokes equations to filter out

all, or at least, parts of the turbulent spectrum. The most widely applied averaging procedure is Reynolds-

averaging (which, for all practical purposes is time-averaging) of the equations, resulting in the Reynolds-

Averaged Navier-Stokes (RANS) equations. By this process, all turbulent structures are eliminated from

the flow and a smooth variation of the averaged velocity and pressure fields can be obtained. However,

the averaging process introduces additional unknown terms into the transport equations (Reynolds

Stresses and Fluxes) that need to be provided by suitable turbulence models (turbulence closures). The

quality of the simulation can depend crucially on the selected turbulence model and it is important to

make the proper model choice as well as to provide a suitable numerical grid for the selected model.

An alternative to RANS are Scale-Resolving Simulation (SRS) models. With SRS methods, at least a portion

of the turbulent spectrum is resolved in at least a part of the flow domain. The most well-known such

method is Large Eddy Simulation (LES), but many new hybrids (models between RANS and LES) are

appearing. As all SRS methods require time-resolved simulations with relatively small time steps, it is

important to understand that these methods are substantially more computationally expensive than

RANS simulations.

ANSYS Fluent provides the following choices of turbulence models:

Spalart-Allmaras model

models

– Standard -  model

– Renormalization-group (RNG) -  model

– Realizable -  model

models

– Standard -

model

– Baseline (BSL) -

model

– Shear-stress transport (SST) -

model

model (add-on)

Transition -

model

Transition SST model

Reynolds stress models (RSM)

– Linear pressure-strain RSM

– Quadratic pressure-strain RSM

– Stress-Omega RSM

– Stress-BSL RSM

Scale-Adaptive Simulation (SAS) model, which can be used in combination with one of the following

based

URANS models:

– SST -

model

model

Modeling Turbulence

– BSL -

model

– Transition SST model

–

based Reynolds stress models (RSM)

Detached eddy simulation (DES) model, which includes one of the following RANS models.

– Spalart-Allmaras RANS model

– Realizable -  RANS model

– SST -

RANS model

– BSL -

RANS model

Shielded Detached Eddy Simulation (SDES) model, which includes one of the following RANS models.

– SST -

RANS model

– BSL -

RANS model

Stress-Blended Eddy Simulation (SBES) model, which includes one of the following RANS models.

– SST -

RANS model

– BSL -

RANS model

Large eddy simulation (LES) model, which includes one of the following subgrid-scale models.

– Smagorinsky-Lilly subgrid-scale model (with or without dynamic stress enabled)

– WALE subgrid-scale model

– Dynamic kinetic energy subgrid-scale model

– Wall-Modeled LES (WMLES)

– Wall-Modeled LES -  (WMLES - )

It is an unfortunate fact that no single turbulence model is universally accepted as being superior for

all classes of problems. The choice of turbulence model will depend on considerations such as the

physics of the flow, the established practice for a specific class of problem, the level of accuracy required,

the available computational resources, and the amount of time available for the simulation. To make

the most appropriate choice of model for your application, you need to understand the capabilities

and limitations of the various options.

Choosing a Turbulence Model

The purpose of this section is to give an overview of issues related to the turbulence models provided

in ANSYS Fluent. The computational effort and cost in terms of CPU time and memory of the individual

models is discussed. While it is impossible to state categorically which model is best for a specific ap-

plication, general guidelines are presented to help you choose the appropriate turbulence model for

the flow you want to model.

Note

For information on turbulence model compatibility with other Fluent models, see Ap-

pendix A: ANSYS Fluent Model Compatibility (p. ).

... Reynolds Averaged Navier-Stokes (RANS) Turbulence Models

... Scale-Resolving Simulation (SRS) Models

... Grid Resolution SRS Models

... Numerics Settings for SRS Models

... Model Hierarchy

RANS models (Reynolds (Ensemble) Averaging in the Theory Guide) offer the most economic approach

for computing complex turbulent industrial flows. Typical examples of such models are the -  or the

models in their different forms. These models simplify the problem to the solution of two addi-

tional transport equations and introduce an Eddy-Viscosity (turbulent viscosity) to compute the Reynolds

Stresses. More complex RANS models are available that solve an individual equation for each of the

six independent Reynolds Stresses directly (Reynolds Stress Models – RSM) plus a scale equation

( -equation or

equation). RANS models are suitable for many engineering applications and typically

provide the level of accuracy required. Since none of the models is universal, you have to decide which

model is the most suitable for a given applications.

.... Spalart-Allmaras One-Equation Model

The Spalart-Allmaras model is a relatively simple one-equation model that solves a modeled transport

equation for the kinematic eddy (turbulent) viscosity. The Spalart-Allmaras model was designed spe-

cifically for aeronautics and aerospace applications involving wall-bounded flows and has been shown

to give good results for boundary layers subjected to adverse pressure gradients. It is also gaining

popularity in turbomachinery applications. Do not use the model as a general purpose model, as it

is not well calibrated for free shear flows (large errors for example, jet flows).

The Spalart-Allmaras model has been extended within ANSYS Fluent with a

insensitive wall treat-

ment, which automatically blends all solution variables from their viscous sublayer formulation to the

corresponding logarithmic layer values depending on

. The blending is calibrated to also cover in-

termediate

values in the buffer layer

.... k-ε Models

Two-equation models are historically the most widely used turbulence models in industrial CFD. They

solve two transport equations and model the Reynolds Stresses using the Eddy Viscosity approach.

The standard -  model in ANSYS Fluent falls within this class of models and has become the workhorse

of practical engineering flow calculations in the time since it was proposed by Launder and Spalding

[] (p. ). Robustness, economy, and reasonable accuracy for a wide range of turbulent flows explain

its popularity in industrial flow and heat transfer simulations.

The draw-back of some -  models is their insensitivity to adverse pressure gradients and boundary

layer separation. They typically predict a delayed and reduced separation relative to observations.

This can result in overly optimistic design evaluations for flows that separate from smooth surfaces

(for example, aerodynamic bodies, diffusers). The -  model is therefore not widely used in external

aerodynamics.

In ANSYS Fluent, the use of the Realizable -  model is recommended relative to other variants of

the -  family. You should use the -  model in combination with either the Enhanced Wall Treatment

(EWT- ) or the Menter-Lechner near-wall treatment. For details, refer to Enhanced Wall Treatment ε-

Equation (EWT-ε) or Menter-Lechner ε-Equation (ML-ε) in the Theory Guide, respectively. For cases

where the flow separates under adverse pressure gradients from smooth surfaces (airfoils, and so on),

models are generally not recommended.

.... k-ω Models

The

equation offers several advantages relative to the -equation. The most prominent one is that

the equation can be integrated without additional terms through the viscous sublayer. This makes

the formulation of a robust

insensitive treatment relatively straightforward. Refer to y+-Insensitive

Wall Treatment ω-Equation in the Theory Guide for details. Furthermore,

models are typically

better at predicting adverse pressure gradient boundary layer flows and separation. The downside

of the standard

equation is a relatively strong sensitivity of the solution depending on the freestream

values of  and

outside the shear layer. The use of the standard -

model is, for this reason, not

generally recommended in ANSYS Fluent.

The BSL and SST -

models have been designed to avoid the freestream sensitivity of the standard

model, by combining elements of the

equation and the -equation. In addition, the SST

model has been calibrated to accurately compute flow separation from smooth surfaces. Within the

model family, it is therefore recommended to use either the BSL or SST model. These models

are some of the most widely used models for aerodynamic flows. They are typically somewhat more

accurate in predicting the details of the wall boundary layer characteristics than the Spalart-Allmaras

model. The BSL and SST models (like all other

equation based models) use the

insensitive wall

treatment by default.

For the -

models, so-called low Reynolds number terms (low Re) have been proposed by Wilcox.

These are available in ANSYS Fluent as an option. It is important to point out that these terms are

not required for integrating the equations through the viscous sublayer. Their main influence lies in

mimicking laminar-turbulent transition processes. However, this functionality is not widely calibrated

and for wall-boundary layer transition, the combination of the SST model with the Transition SST

model (Transition SST Model in the Theory Guide), Intermittency Transition model (Intermittency

Transition Model in the Theory Guide), or the Transition -

model (k-kl-ω Transition Model in the

Theory Guide) is more reliable. The use of the low-Re terms is therefore not encouraged.

.... Generalized k-ω (GEKO) Model

The goal of the GEKO model is to offer a single model with enough flexibility to cover a wide range

of applications. Although most applications are already covered by the default settings, the model

provides four free parameters that can be adjusted for specific types of applications, without negative

impact on the basic calibration of the model. This is a powerful tool for model optimization, but requires

a proper understanding of the impact of these coefficients to avoid mistuning. It is important to

emphasize that the model has strong defaults, so you can also apply the model without any fine-

tuning and that you should make sure that any tuning is supported by high-quality experimental

data.

data.

In most cases, you need to only adjust

to change the GEKO model’s sensitivity to boundary

layer separation. The figure below shows the impact of this parameter for a diffuser flow [] (p. ).

With

, the model behaves essentially the same as the

model (no separation) and with

, close to perfect agreement with the data is achieved (like the SST model [] (p. )).

Larger values for

can be required (for example, when simulating high-lift airfoils, where even

the SST model tends to under-estimate separation strength).

Figure . : Velocity Profiles for Axi-symmetric Diffuser Flow (Case CS0 – Driver). Impact of

Variation of

The figure below shows variations of

for a free mixing layer (

) [] (p. ). Increasing

leads to increased turbulence levels and larger spreading rates.

Figure . : Impact of Changes in

on Free Mixing Layer. Left: Velocity Profiles, Right:

Turbulence Kinetic Energy Profiles

The impact of

is shown in the figure below for the reattachment region of a backward-facing

step [] (p. ). Both the wall shear stress coefficient

and the Stanton number for heat transfer,

, are strongly affected. Increasing

leads to higher

and

numbers in this non-equilibrium

region. In most cases, there is no need to change

from its default value.

on Backward Facing Jet with Heat Transfer. Left: Wall

Shear Stress Coefficient,

, Right: Wall Heat Transfer Coefficient,

The figure below shows the influence of

for plane [] (p. ) and round jet flows

[] (p. )(

=,

=.,

=.). Increasing

(while

is active) reduces the

[] (p. )(

=,

=.,

(while

spreading rate for jet flows without changing the spreading rate of mixing layers.

is a sub-

model of

and therefore loses its effectiveness in cases where

is reduced.

on Free Jet Flows. Left: Plane Jet, Right: Round Jet

Note that the region where

is active is defined by the blending function

. In regions where

= (near walls) there is no effect when changing

.

can be visualized in the Post

Processor. It can also be augmented by the modification of expert parameters (see Generalized k-ω

(GEKO) Model in the Fluent Theory Guide) or by over-writing the function via a UDF (see

DEFINE_KW_GEKO Coefficients and Blending Function in the Fluent Customization Manual).

.... Reynold Stress Models

Reynolds Stress models (RSM) include several effects that are not easily handled by Eddy-Viscosity

models. The most important effect is the stabilization of turbulence due to strong rotation and

streamline curvature (as observed for example, in cyclone flows). RSM on the other hand often demand

a significant increase in computing time partly due to the additional equations but mostly due to

reduced convergence. This additional effort is not always justified by increased accuracy. Their usage

is therefore not generally recommended and should be restricted to flows for which their superiority

has been established, especially flow with strong swirl and rotation. If wall boundary layers are im-

portant, the combination of RSM with the

or BSL-equation is more accurate than the combination

with the -equation. The combination of RSM with BSL removes the free-stream sensitivity observed

with the

equation in the same way as for two-equation models.

.... Laminar-Turbulent Transition Models

The following three models for transition prediction are available in ANSYS Fluent. Two of them can

be combined with the scale-resolving methods described in Scale-Resolving Simulation (SRS) Mod-

els (p. ).

the Transition SST model (also known as the -

model)

This model can be combined with Scale-Adaptive Simulation, Detached Eddy Simulation, Stress-

Blended Eddy Simulation, and Shielded Detached Eddy Simulation.

the Intermittency Transition model (also known as the  model, and available for BSL, SST, Scale-Adaptive

Simulation with BSL / SST, Detached Eddy Simulation with BSL / SST, Stress-Blended Eddy Simulation with

BSL / SST, and Shielded Detached Eddy Simulation with BSL / SST)

the Transition -

model

For many test cases, the three models produce similar results. Due to their combination with the SST

model, the Transition SST model and the Intermittency Transition model are recommended over the

model. The Transition SST model is not Galilean invariant, and should therefore not

be applied to surfaces that move relative to the coordinate system for which the velocity field is

computed; furthermore, it is not suitable for fully developed pipe / channel flows where no freestream

is present. For such cases, the Intermittency Transition model should be used instead (though you

may need to adjust the Intermittency Transition model for pipe / channel flows by modifying the

underlying correlations). Among the three models, only the Intermittency Transition model is capable

of accounting for crossflow instability.

When using these models, note the following:

These models are only applicable to wall-bounded flows. Like all other engineering transition models,

they are not applicable to transition in free shear flows.They will predict free shear flows as fully turbulent.

These models have not been calibrated in combination with other physical effects that affect the source

terms of the turbulence model, such as:

– buoyancy

– multiphase turbulence

No special calibration has been performed for the combination of the Transition SST and Intermittency

Transition model with scale-resolving methods.

Note that the activation of the LES term in the freestream in any hybrid RANS-LES model can affect

the decay of the freestream turbulence, which in turn affects the transition location.

Proper mesh refinement and specification of inlet turbulence levels is crucial for accurate transition pre-

diction.

In general, there is some additional effort required during the mesh generation phase because a low-Re

mesh with sufficient streamwise resolution is needed to accurately resolve the transition region. Further-

more, in regions where laminar separation occurs, additional mesh refinement is necessary in order to

properly capture the rapid transition due to the separation bubble.

The decay of turbulence from the inlet to the leading edge of the device should always be estimated before

running a solution as this can have a large effect on the predicted transition location. Physically correct

values for the turbulence intensity (Tu) should be achieved near the location of transition.

.... Curvature Correction for the Spalart-Allmaras and Two-Equation Models

One weakness of the eddy-viscosity models is that these models are insensitive to streamline curvature

and system rotations, which play an important role in many turbulent flow applications. To sensitize

the standard eddy-viscosity models to these curvature effects, you can use a modified turbulence

production term. For more information, see Curvature Correction for the Spalart-Allmaras and Two-

Equation Models in the Fluent Theory Guide.

.... Production Limiters for Two-Equation Models

A disadvantage of standard two-equation turbulence models is the excessive generation of the tur-

bulence energy,

, in the vicinity of stagnation points. In order to avoid the buildup of turbulent

kinetic energy in the stagnation regions, the production term in the turbulence equations can be

limited by one of the two formulations described in Production Limiters for Two-Equation Models in

the Fluent Theory Guide.

.... Model Enhancements

There are many model enhancements available for turbulence models. While such enhancements can

improve simulations in some cases, they can also have detrimental effects. The general recommend-

ation is therefore to use them with caution.

As noted above, the use of low-Re terms in combination with the

equation is not generally recom-

mended.

mended.

Another model enhancement that should be used with care is the compressibility effects of Sarkar

([] (p. )). It can improve the prediction of free shear layers at high Mach numbers, but has also

shown a pronounced negative impact on wall boundary layers. It is therefore not generally recom-

mended. The compressibility effects option is available in the Viscous Model Dialog Box (p. ) when

the compressible form of the ideal gas law or the real-gas model is enabled. This option is disabled

by default (though this was not the case in version . and earlier) and it is recommended that you

keep this option disabled for cases not involving free shear flows.

Buoyancy has a pronounced effect on turbulence (Effects of Buoyancy on Turbulence in the Theory

Guide). The use of the source term in the -equation is therefore recommended for buoyancy affected

flows. The source term in the -equation and

equation is much less established and the term should

be enabled with care.

....Wall Treatment for RANS Models

It is recommended that you use a

insensitive wall treatment for all models for which it is available

(Spalart-Allmaras, -equation and

equation). It provides the most consistent wall shear stress and

wall heat transfer predictions with the least sensitivity to

values. (See an Overview of the Spalart-

Allmaras model, Enhanced Wall Treatment ε-Equation (EWT-ε), Menter-Lechner ε-Equation (ML-ε), and

y+-Insensitive Wall Treatment ω-Equation in the Theory Guide for more information.)

When Wall Functions are used, it is necessary to avoid grids with fine near wall spacing. It is recom-

mended that you use

in the entire domain. The application of Wall Functions is, however, not

generally recommended as they do not allow a systematic refinement of the near wall grid. Wall

Functions are especially damaging for flows at low to medium Reynolds numbers (Re~

), as

the assumption of an extended logarithmic layer is not valid in these cases. In case that Wall Functions

are desired, the option of Scalable Wall Functions (Scalable Wall Functions in the Theory Guide) avoids

the grid restrictions and can be run on fine meshes.

.... Grid Resolution for RANS Models

Grid generation has a strong impact on model accuracy. There are many considerations that have to

be followed when generating high quality CFD grids. From a turbulence modeling standpoint, the

most important one is that the relevant shear layers should be covered by at least ~ cells normal

to the layer. Below this resolution, the model will not be able to provide its calibrated performance.

Especially for free shear flows, whose location is not known during grid generation, this is a requirement

that is hard to achieve. Nevertheless, you should be aware that for lower resolution, the model per-

formance can degrade.

For wall bounded flows, a structured mesh in wall-normal direction is highly recommended. The

structured portion of the mesh should cover the entire boundary layer and extend beyond the

boundary layer thickness to avoid restricting the growth of the boundary layer. Advanced turbulence

models for wall boundary layers like the Spalart-Allmaras model and the SST model will only provide

improved results to other models if a minimum of  or more structured (hex or prism) cells are located

inside the boundary layer. In addition, one should ensure that the prism layer covers the wall

boundary layer entirely. Note that these are not specific requirements of these models, but are gen-

eral requirements for wall boundary layer simulations.

Both ε-based and ω-based models offer

insensitive wall treatment options (see Enhanced Wall

Treatment ε-Equation (EWT-ε), Menter-Lechner ε-Equation (ML-ε), and y+-Insensitive Wall Treatment

ω-Equation in the Theory Guide for more information), which make the models relatively insensitive

to the

value of the wall cell. Generally speaking, it is more important to ensure that the boundary

layer is covered with sufficient cells, then to achieve a certain

criterion. However, for simulations

with high accuracy demands on the wall boundary layer (especially for heat transfer predictions),

near-wall meshes with

~ are recommended. When wall functions are used, it is essential to avoid

meshes with

values lower than ~ as the wall shear stress and the wall heat transfer can and will

seriously deteriorate under such conditions. For this reason, the usage of

insensitive wall treatments

(to be selected for -equation and default for

equation based models) is recommended.

For transition models (see k-kl-ω Transition Model, Transition SST Model, and Intermittency Transition

Model in the Theory Guide), more stringent grid resolution requirements apply than for standard

RANS models, as transition modeling requires the resolution of the thin laminar boundary layer up-

stream of the transition location. For this reason, a low-Re mesh (

) with sufficient streamwise

resolution is needed to accurately resolve the transition region. The expansion ratio of the grid normal

to the wall should not exceed .. Furthermore, in regions where laminar separation occurs, additional

mesh refinement is necessary, in order to properly capture the rapid transition due to the separation

bubble. Finally, the decay of turbulence from the inlet to the leading edge of the device should always

be estimated before running a solution as this can have a large effect on the predicted transition

location.

The alternative to RANS models are models that resolve at least a portion of the turbulence for at least

a portion of the flow domain. Such models are generally termed ‘Scale-Resolving’.

.... Large Eddy Simulation (LES)

The most widely known SRS modeling concept is Large Eddy Simulation (LES). It is based on the ap-

proach of resolving large turbulent structures in space and time down to the grid limit everywhere

in the flow. However, while widely used in the academic community, LES had very limited impact on

industrial simulations. The reason lies in the excessively high resolution requirements for wall

boundary layers. Near the wall, the largest scales in the turbulent spectrum are nevertheless geomet-

rically very small and require a very find grid and a small time step. In addition, unlike RANS, the grid

cannot only be refined in the wall normal direction, but also must resolve turbulence in the wall

parallel plane. This can only be achieved for flows at very low Reynolds number and on very small

geometric scales (the extent of the LES domain cannot be much larger than - times the

boundary layer thickness parallel to the wall). For this reason the use of LES is only recommended

for flows where wall boundary layers are not relevant and need not be resolved or for flows where

the boundary layers are laminar due to the low Reynolds number. In such cases, the most balanced

LES model is the WALE model (see Wall-Adapting Local Eddy-Viscosity (WALE) Model in the Theory

Guide). It offers a good compromise between model complexity and generality. It also allows computing

laminar shear (boundary) layers without any model impact.

An extension to LES is Wall-Modeled LES (WMLES). It allows the LES computation of wall bounded

flows at higher Reynolds number without the large increase in grid resolution required for conven-

tional LES at high Reynolds numbers. For WMLES, the grid resolution is largely independent of the

Reynolds number with respect to the grid cells required per boundary layer volume. An enhanced

version of WMLES called WMLES -  is also available. WMLES does not provide zero eddy-viscosity

for flows with constant shear. Therefore, it does not allow the computation of transitional effects, and

can produce overly large eddy-viscosities in separating shear layers. The enhanced WMLES -  for-

mulation overcomes these deficiencies. See Algebraic Wall-Modeled LES Model (WMLES) in the Theory

Guide for further details.

.... Hybrid RANS-LES Models

In order to avoid the high resolution requirements of LES, numerous hybrid models have been de-

veloped in recent years. These are models that combine certain elements of RANS and LES approaches

in a way that allows for the simulation of high Reynolds number flows. With hybrid models, the at-

tached wall boundary layers are typically covered by the RANS part of the model, while large detached

regions are handled in ‘LES’ mode, meaning with a partial resolution of the turbulent spectrum in

space and time. Hybrid models rely on a strong enough flow instability to generate turbulent structures

in the separated zone. This is typically the case for flows behind bluff bodies, where URANS models

predict single-mode periodic vortex shedding. Hybrid models allow these vortices to generate smaller

eddies down to the available grid limit. Figure . : Illustration of SST-URANS vs. SST-SAS Models (p. )

shows a typical scenario: While the application of a standard RANS model in unsteady mode results

in a single frequency vortex shedding (left), the application of hybrid models allows a break-up of

the large structures into smaller scales. This is beneficial for predicting the correct mixing behind the

body or to extract spectral information (for example, for acoustic simulations). At the same time, the

wall boundary layers are covered by the RANS part of the hybrid model avoiding the excessive resol-

ution requirements of LES.

Figure . : Illustration of SST-URANS vs. SST-SAS Models

Figure . : Illustration of SST-URANS vs. SST-SAS Models (p. ) shows a circular cylinder in a cross

flow at

. The left hand side illustrates the SST-URANS model, while the right-hand side

illustrates the SST-SAS model. The isosurface of

is colored according to the eddy viscosity

ratio

(note that the scale in the right-hand side figure is smaller by a factor of ).

..... Scale-Adaptive Simulation (SAS)

The SAS modeling approach (see Scale-Adaptive Simulation (SAS) Model in the Theory Guide) as

proposed by Menter et al. ([] (p. ) [] (p. )) is based on the introduction of the von Karman

length scale,

, into the turbulence equations (for the BSL and SST models, it enters into the

equation).

is defined as the ratio of the first divided by the second derivative of the velocity

vector (times the von Karman constant =. ):

(.)

The inclusion of this term allows the model to adjust its length scale to already resolved scales in

the flow and thereby provide a low enough eddy viscosity to allow the model to operate in ‘LES’

mode.

The SAS approach has the advantage that the RANS part of the model is unaffected by the grid

spacing and will therefore not allow a deterioration of model accuracy as seen in DES in regions of

refined grid but insufficient flow instability. However, in cases where the flow instability is not strong

enough, the SAS will remain in RANS mode and will not produce unsteady structures. While this is

often a sign that the RANS model is still reasonably capable of handling the flow, it is a limitation if

unsteady information is required (for example, in acoustics). In such cases, the internal interface

option of the ELES implementation can be applied to convert modeled turbulence into resolved

turbulence (see Internal Interface Without LES Zone in the Theory Guide).

..... Detached Eddy Simulation (DES)

The DES model (see Detached Eddy Simulation (DES) in the Theory Guide) achieves the switch

between RANS and LES by a comparison of the turbulent length scale

with the grid spacing

.

The model selects the minimum of both and thereby switches between RANS and LES mode by re-

placing  in the -equation by:

(.)

Once the model selects the grid spacing as the minimum, the model is operating in ‘LES’ mode.

The grid spacing enters explicitly into the DES model. This can affect the RANS solution in regions,

where the grid is between RANS and LES resolution (so-called ‘gray zones' in DES) and/or where the

flow instability is not strong enough to generate LES structures. Another issue to consider with DES

is the problem of ‘grid-induced-separation’ (GIS). It occurs if the grid for an attached wall boundary

layer flow is refined to a point where the DES limiter becomes active and affects the RANS solution.

However, in such situations, the flow instability is not strong enough to balance the reduced RANS

content by resolved turbulence. This will typically result in an artificial flow separation at the location

of grid refinement. It typically happens if

(  being the boundary layer thickness). Remedies

for this situation have been proposed by Menter et al. who recommended using the F1 blending

function of the SST-DES model to shield the boundary layers from the DES limiter. Later, alternative

blending functions for the same purpose have been proposed by Spalart et al. ([] (p. ))—res-

ulting in the terminology Delayed DES (DDES). The DDES model as originally proposed for the Spalart-

Allmaras model provided limited protection against GIS for two-equation models such as BSL, SST,

and - . Therefore, the DDES function has been re-calibrated for the BSL, SST, and -  models and

is now the recommended choice and the default setting when using these models.

A further refinement is provided by the Improved DDES (IDDES) formulation of Strelets et al.

([] (p. )), which extends the LES zone of the model to the outer part of wall boundary layers.

This allows the simulation of wall boundary layers in Wall-Modeled LES (WMLES) mode. In this

model, the IDDES model is applied like a LES model, typically with the specification of unsteady inlet

conditions. The grid resolution requirements for WMLES are much less stringent than for LES.

All of the above shielding function variants are available in ANSYS Fluent. For the Spalart-Allmaras

model, the original DDES shielding function is used. For the - , BSL, and SST models, the DDES

function has been re-calibrated for better boundary layer protection. The re-calibrated DDES function

is the default selection and is recommended over the use of the F1 or F2 functions for the BSL / SST

model. Despite the potential difficulties in the application of hybrid methods, they have the potential

to greatly expand the usage of Scale-Resolving Simulation models for engineering applications, as

they avoid the excessive resolution required by LES for wall boundary layers. IDDES in WMLES mode

is an advanced option and should only be used if you are familiar with the original literature and

the grid requirements for this model.

The DES and DDES models in ANSYS Fluent have been superseded by the SDES and SBES models

described in Shielded Detached Eddy Simulation (SDES) and Stress-Blended Eddy Simulation

(SBES) (p. ).

..... Shielded Detached Eddy Simulation (SDES) and Stress-Blended Eddy Simulation

(SBES)

The Shielded Detached Eddy Simulation (SDES) model and the Stress-Blended Eddy Simulation (SBES)

model are hybrid RANS-LES models with an improved shielding function compared to DDES / IDDES.

They provide strong shielding of the RANS boundary layer, faster “transition” from RANS to LES in

separating shear layers, and (for SBES) explicit selection of the LES model. For implementation details,

see Shielded Detached Eddy Simulation (SDES) and Stress-Blended Eddy Simulation (SBES) in the

Theory Guide; for setup details, see Including the SDES or SBES Model with BSL, SST, and Transition

SST Models (p. ).

These models are recommended over the older DES / DDES model formulations. The SBES model is

considered the optimal selection, as it offers the clearest distinction between RANS and LES zones.

.... Zonal Modeling and Embedded LES (ELES)

As pointed out in the previous sections, hybrid models rely on flow instabilities to generate turbulent

structures in large separated regions without the explicit introduction of unsteadiness through the

boundary conditions. However, there are situations, where such instabilities are not present or are

not reliable to serve this purpose. In such cases, it is desirable to apply RANS and the LES models in

predefined zones and provide clearly defined interfaces between them. At these interfaces, the

modeled turbulent kinetic energy from the upstream RANS model is converted explicitly to resolved

scales at an internal boundary to the LES zone. The LES zone can then be limited to the region of

interest where unsteady results are required. ELES is available in ANSYS Fluent and allows the com-

bination of most RANS model with classical LES models. It is important to emphasize that in this

mode, a full LES resolution is required within the LES zone. In the LES zone, using the WALE model

is recommended (see Wall-Adapting Local Eddy-Viscosity (WALE) Model in the Theory Guide).

Grid Resolution SRS models are discussed in the following sections:

....Wall Boundary Layers

.... Free Shear Flows

For wall boundary layers, it is important to distinguish if they are computed in RANS or wall-resolved

or Wall-Modeled LES (WMLES) mode. Only the IDDES and the SBES model can be run in WMLES mode

reliably.

In the case of RANS mode, the requirements are the same as for any RANS model. For a wall-resolved

LES, it is typically recommended to use a mesh with a grid spacing scaling with

where x is the streamwise, y the wall normal and z the spanwise direction (for example, channel flow).

However, in complex applications, the distinction between streamwise and spanwise direction is not

feasible and then

would be required. This scaling demonstrates the strong

Reynolds number dependency of the LES approach for wall bounded flows.

For the IDDES and SBES models in WMLES mode, the above requirements can be relaxed. The grid

spacing no longer scale with the wall friction, but with the boundary layer thickness . It is recom-

. The wall normal resolution should be like for a finely

resolved RANS simulation, meaning a near wall resolution of

and around  nodes inside the

boundary layer.

For free shear flows, it is difficult to provide general recommendations, as there are many different

flow scenarios. The current recommendation is therefore based on the most common (and most fre-

quent) free shear flow – a turbulent mixing layer. It will not necessarily apply to other free shear flows

like jets and you are advised to perform tests as to the optimal resolution of your specific flow.

For free shear flows and SRS models, one should aim for uniform isotropic cells (all edges have similar

length). The shear layer should be covered by ~- cells.

For Scale-Resolving Simulations (SRS), specific discretization and solver settings are required to achieve

optimal accuracy with minimal numerical effort. The recommendations given below should be considered

as a starting point for your specific flow application and are not generic, but problem dependent. The

recommendations are based on incompressible, single phase flow without chemical reactions or other

complex additional physics. In case your simulation features additional complex physical effects, it re-

quires adjusting the recommended solver settings accordingly. In most cases, this will mean that a

higher effort must be invested into the coupling of the equations (for example lower time step, reduced

under-relaxation, higher iteration count, smaller residuals), in order to avoid a de-coupling of different

physical phenomena.

For Scale-Resolving Simulations, optimal numerics settings are essential for achieving accurate results

in an acceptable time frame. The reason is that at the SRS models operate at the resolution limit of

the provided grid where the smallest scales are of the order of the grid spacing and the time resolution.

Numerics settings therefore have to be chosen to provide an optimal balance between accuracy and

robustness.

It is generally recommended to initialize the solution from a (reasonably) converged RANS simulation.

....Time Discretization

For Scale-Resolving Simulations, the resolution of the turbulent structures in time is essential for the

success of the simulation. This is, to the largest extent, defined by the selected time step. As the SRS

model is operating at the grid limit, you should select a time step that ensures a Courant-Friedrichs-

Levy (CFL) number of

(.)

The CFL number is computed by the solver and can be checked based on an initial RANS simulation,

for example. It is important to emphasize that this is not a numerical limit and that the solver will be

able to sustain much larger CFL numbers. In complex applications, there will always be limited regions

of fine cells or large velocities and you should not restrict the CFL number based on such zones. The

recommendation of CFL = should be applied in the main SRS region in combination with a uniform

isotropic grid. It is recommended that you vary the time step for each type of application and explore

its optimal value. This can substantially save on computing costs.

The time derivative should be computed by the Second Order Implicit option. (See User Inputs for

Time-Dependent Problems (p. ) for guidelines on setting solution parameters for transient calcula-

tions in general.)

.... Spatial Discretization

For SRS models, it is important to minimize the numerical dissipation of the scheme in order to avoid

damping of the smallest scales by numerical dissipation. For the pressure-based solver, the choice

for spatial discretization is between the Central Differencing (CD) scheme (see Central-Differencing

Scheme in the Theory Guide) and the Bounded Central Differencing scheme (BCD) (see Bounded

Central Differencing Scheme in the Theory Guide); for the density-based solver, BCD is available with

the Roe-FDS or AUSM flux type for the discretization of the flow equations, but CD is not. The Central

Differencing scheme is the least dissipative and provides the highest resolution accuracy for the

smallest scales. Especially for aero-acoustics simulations, where the spectral content at higher frequen-

cies can be important, this is a desirable feature. However, Central Differencing schemes are prone

to solution oscillations (checker boarding) in the velocity field. When using the Central Differencing

scheme, it is therefore important to provide a high quality mesh (no mesh jumps, isotropic cells and

high resolution in critical zones) and to avoid large time steps (the CFL number should be smaller

than  in the main SRS region). It is recommended that you visually monitor the solution regularly in

order to avoid wasting computational resources. In case oscillations appear, the choice is to: improve

the mesh; reduce the time step; or to switch to the slightly more dissipative, but also more robust

Bounded Central Differencing scheme. In many complex applications, the Bounded Central Differencing

Scheme is the numerics option of choice. It typically provides sufficiently low dissipation to allow the

turbulent structures to evolve, but, at the same time, is robust enough to handle non-optimal grids

as they are typically encountered in industrial simulations. In addition, the Bounded Central Differencing

scheme is also suitable for hybrid methods like SAS, DES, SDES, and SBES, and will provide stable

solutions in RANS regions, with highly stretched grids and with a CFL number larger than . For ELES,

the numerical scheme in the LES zone can be selected independently from the settings in the RANS

zone. The RANS region can then be computed with standard higher-order upwind schemes and the

LES zone can be covered by either the Central Differencing scheme or the Bounded Central Differencing

scheme.

For the gradient calculation, it is recommended that you select the Least Squares Cell Based option,

or the Green-Gauss Node Based option, to ensure a second-order interpolation on non-orthogonal

grids.

grids.

For pressure interpolation, it is recommended that you use the second-order scheme, or the body-

force-weighted scheme. Due to its higher dissipation, the PRESTO! scheme (see Pressure Interpolation

Schemes in the Theory Guide) can result in a delayed formation or damping of turbulent structures.

It is therefore not recommended for SRS.

.... Iterative Scheme

The selection of the iterative scheme will mostly affect the computational costs as the cost per iteration

between these methods is rather different. However, recommendations are not straightforward, as

the higher cost per iteration of a scheme can be offset by faster convergence within the time step.

The fastest scheme is the Non-Iterative Time Advancement (NITA) scheme (see Non-Iterative Time-

Advancement Scheme in the Theory Guide  as well as Setting Solution Controls for the Non-Iterative

Solver (p. )). This scheme typically works well for limited LES zones and high quality meshes. It is

also important to ensure a low time step of a CFL number below . For the NITA scheme, all explicit

under-relaxation factors are, by default, set equal to one. With NITA, it has slight advantages to use

the fractional step method if there is no involvement of more complex physics, when otherwise the

PISO scheme can be more beneficial. Note that with the LES model, you can enable an accelerated

time marching option, which enables a modified NITA scheme and other setting changes that can

further speed up the simulation; for details, see Setting Solution Controls for the Non-Iterative Solv-

er (p. ).

In case the application is too complex for the NITA scheme to provide a solution, the iterative SIMPLEC

er (p. ).

(SIMPLE vs. SIMPLEC (p. )) or PISO (PISO (p. )) schemes are the next possible option. They should

be preferred relative to the SIMPLE scheme, as they show faster convergence per time step and can

be run with more aggressive under-relaxation (higher values equal to  or close to ). If such settings

prevent convergence within the time step, then check if your time step is small enough for maintaining

CFL numbers below  in the SRS region – if not, then try reducing

. If this is not possible, or does

not lead to satisfactory convergence, then reduce the under-relaxation factors to values between the

default settings and . For skewed meshes or meshes with problematic quality, the reduction of ex-

plicit relaxation factor for pressure correction down to . from  can be very helpful.

..... Convergence Control

The convergence criterion within each time step will strongly affect solution costs, as a low criterion

will result in an increased number of iterations. It is not possible to provide general recommendations,

as the required residual depends on the application. The most relevant residual in the SRS models

is the continuity residual. It should be converged by approximately  orders of magnitude per time

step for a CFL number ~ . This should be achievable with around - maximum iterations per time

step for flows involving no other physical models. Be sure to check the impact of convergence on

your solution to ensure that the residual is reduced to a level consistent with your problem.

For simulations with small CFL values, the Extrapolate Variables option (available in the Run Calcu-

lation Task Page (p. )) can be very beneficial. This can substantially reduce the number of iterations

within the time step up to % when the convergence control is based on the convergence criteria.

In case your simulation requires the combination of additional physical models, such as combustion

or multiphase, a reduction of the under-relaxation factors might be required. In this case, the number

of maximum iterations per time step can be increased to achieve the desired residual reduction.

For hybrid RANS/LES simulations, such as the SAS, DES, SDES, and SBES models, there can be situations

where the RANS portion of the flow limits convergence (for example, due to poor grid quality). In

such cases, the application of the coupled solver should be considered. For the coupled pressure-

based solver, each iteration is typically more expensive than for the SIMPLEC algorithm, but this is

at least partly offset by faster convergence. The recommendations concerning residuals are similar

to the SIMPLEC method, but the maximal number of iterations can be reduced to values as low as

for highly unstable flows, and - for more sensible flows and acoustics simulations.

As discussed, turbulence modeling is a balance between accuracy and cost. The recommendation is

to use RANS models as much as possible and as long as they provide the accuracy required for the

simulation. RANS models will remain the workhorse of turbulence modeling for many years to come.

Within the RANS family, eddy-viscosity models are typically sufficient for most engineering flow simu-

lations. The application of RSM is only recommended for flows that are known to systematically benefit

from their usage and justify the increase in computing power.

In cases where steady RANS or URANS models cannot provide the accuracy or unsteady information

required, it is recommended that you switch to the SAS approach. It is relatively forgiving in terms of

the grid resolution and will not deteriorate the results in case of insufficient resolution in the unsteady

zone. The SAS model will only provide scale-resolution if a strong flow instability is present. Visual in-

spection (using isosurfaces of the Q criterion) will quickly allow a judgment if the model provides suf-

ficient unsteadiness and resolution relative to the grid spacing. In such cases, the internal interface

option of the ELES implementation can be applied to convert modeled turbulence into resolved tur-

bulence (see Internal Interface Without LES Zone in the Theory Guide).

DDES (DES is not recommended) models can allow the formation of unsteadiness even for cases where

SAS remains stable. DDES does require a more carefully crafted grid in the LES zone due to the DES

grid influence on the RANS solution. For the DES-BSL / SST model, use the default DDES blending

function for shielding.

SDES and SBES have an improved shielding function compared to DDES / IDDES. They provide strong

shielding of the RANS boundary layer and demonstrate a fast “transition” between RANS and LES in

separating shear layers. The SBES model formulation in combination with the WALE LES model is re-

commended over older models like DES, DDES, and IDDES.

ELES is recommended in cases where limited zones with high accuracy requirements are embedded

inside a larger RANS zone. At the interface between the RANS and the LES zone, unsteady turbulence

is generated either by the Vortex Method or the Spectral Synthesizer. For wall bounded flows, the ELES

method requires a very fine near wall resolution in the LES zone.

Pure LES should only be applied to free shear flows (for example, combustion chambers without wall

influence) or to very limited domains using meshes with fine LES near wall resolution. It is important

to be aware of the strong increase of grid resolution requirements with Reynolds number for wall

bounded flows. For wall boundary layers at higher Reynolds numbers, the IDDES model can be run in

WMLES mode – meaning with specified unsteady inlet conditions.

When your ANSYS Fluent model includes turbulence you need to enable the relevant model and options,

and supply turbulent boundary conditions. These inputs are described in this section.

The procedure for setting up a turbulent flow problem is described below. (Note that this procedure

includes only those steps necessary for the turbulence model itself; you will need to define the other

settings—for example, other models, boundary conditions—as usual.)

. Define the turbulence model settings.

a.

a.

Open the Viscous Model Dialog Box (p. ) (Figure . :The Viscous Model Dialog Box (p. )) by right-

clicking Viscous in the tree (under Setup/Models) and clicking Edit... in the menu that opens.

Edit...

Figure . : The Viscous Model Dialog Box

b. Select either Spalart-Allmaras, k-epsilon, k-omega, Transition k-kl-omega, Transition SST, Reynolds

Stress, Scale-Adaptive Simulation (SAS), Detached Eddy Simulation (DES), or Large Eddy Simulation

(LES) from the Model list.

Steps in Using a Turbulence Model

If you choose the k-epsilon model, select either Standard, RNG, or Realizable from the k-epsilon

Model list. If you choose the k-omega model, select Standard, BSL, or SST from the k-omega

Model list.

Important

The Large Eddy Simulation (LES) model is available only for 3D cases.

c.

If the flow involves walls, and you are using one of the -  models or the -based Reynolds stress

models, choose one of the following options from the Near-Wall Treatment list in the Viscous Model

Standard Wall Functions

Scalable Wall Functions

Non-Equilibrium Wall Functions

Enhanced Wall Treatment

Menter-Lechner (for -  models only)

User-Defined Wall Functions

For more information about these near-wall options, see Near-Wall Treatments for Wall-Bounded

Turbulent Flows in the Theory Guide. By default, the standard wall function is enabled.

For more information about the automatically defined near-wall treatment for the Spalart-Allmaras

model, see Wall Boundary Conditions in the Theory Guide.

For more information about the automatically defined near-wall treatment for the -

model,

model,

see Wall Boundary Conditions in the Theory Guide.

For more information about the automatically defined near-wall treatment and the optional

Werner-Wengle near-wall treatment for the LES model, see Inlet Boundary Conditions for Scale

Resolving Simulations and LES Near-Wall Treatment in the Theory Guide, respectively.

d. Enable the other appropriate turbulence modeling options in the Viscous Model dialog box, as appro-

priate. See Setup Options for All Turbulence Modeling (p. )

. Specify the boundary conditions for the solution variables in the appropriate boundary condition dialog

boxes.The boundary condition dialog boxes can be opened by right-clicking the boundary name in the

tree (under Setup/Boundary Conditions) and clicking Edit... in the menu that opens; alternatively, you

can open them from the Boundary Conditions task page:

Setup →

See Defining Turbulence Boundary Conditions (p. ) for details.

. Specify the initial guess for the solution variables in the Solution Initialization task page.

Solution →

See Providing an Initial Guess for k and ε (or k and ω) (p. ) for details. Note that Reynolds stresses

are automatically initialized using , and therefore need not be initialized explicitly.

If you choose the Spalart-Allmaras model, the following options are available:

vorticity-based production (Vorticity- and Strain/Vorticity-Based Production (p. ))

strain/vorticity-based production (Vorticity- and Strain/Vorticity-Based Production (p. ))

viscous heating (always enabled for the density-based solvers) (Including the Viscous Heating Effects (p. ))

curvature correction (Including the Curvature Correction for the Spalart-Allmaras and Two-Equation Turbu-

lence Models (p. ))

Figure . : The Viscous Model Dialog Box Displaying the Spalart-Allmaras Production

Setting Up the k-ε Model

... Setting Up the Standard or Realizable k-ε Model

... Setting Up the RNG k-ε Model

If you choose the standard -  model or the realizable -  model, the following options are available:

inclusion of buoyancy effects on  (see Effects of Buoyancy on Turbulence in the k-ε Models in the Theory

Guide)

inclusion of curvature correction (Including the Curvature Correction for the Spalart-Allmaras and Two-

Equation Turbulence Models (p. ))

inclusion of compressibility effects (Including the Compressibility Effects Option (p. ))

inclusion of production limiters (Including Production Limiters for Two-Equation Models (p. ))

Figure . : The Viscous Model Dialog Box Displaying the Standard k-ε Model

For all -  models, one of the following near-wall treatments must be selected (see Near-Wall Treatments

for Wall-Bounded Turbulent Flows in the Theory Guide):

standard wall functions

scalable wall functions

non-equilibrium wall functions

enhanced wall treatment

Menter-Lechner

user-defined wall functions

If you choose the enhanced wall treatment, the following options are available:

pressure gradient effects (Including Pressure Gradient Effects (p. ))

thermal effects (Including Thermal Effects (p. ))

If you select user-defined wall functions for the near-wall treatment, hook your UDF using the Law of

the Wall drop-down list that appears at the bottom of the User-Defined Functions group box in the

Viscous Model dialog box.

If you choose the RNG -  model, the following options are available:

differential viscosity model (Differential Viscosity Modification (p. ))

swirl modification (Swirl Modification (p. ))

Guide)

Figure . : The Viscous Model Dialog Box Displaying the RNG k-ε Model

... Setting Up the Standard k-ω Model

... Setting Up the Baseline (BSL) k-ω Model

... Setting Up the Shear-Stress Transport k-ω Model

... Setting up the Generalized k-ω (GEKO) Model

If you choose the standard -

model, the following options are available:

low-Re corrections (Low-Re Corrections (p. ))

shear flow corrections (Shear Flow Corrections (p. ))

turbulence damping (available with the VOF and Mixture models and the Eulerian multiphase model when

using the Multi-Fluid VOF model) (Turbulence Damping (p. ))

Setting Up the k-ω Model

a scale-resolving simulation option: Scale-Adaptive Simulation (Setting Up Scale-Adaptive Simulation (SAS)

Modeling (p. ))

Figure . : The Viscous Model Dialog Box Displaying the Standard k-ω Model

The -

models use

insensitive near-wall treatment (see y+-Insensitive Wall Treatment ω-Equation

If you choose the baseline (BSL) -

inclusion of the Intermittency Transition model

scale-resolving simulation options: either Scale-Adaptive Simulation (Setting Up Scale-Adaptive Simulation

(SAS) Modeling (p. )), Detached Eddy Simulation (Setting Up DES with the Transition SST Model (p. )),

Stress-Blended Eddy Simulation (Including the SDES or SBES Model with BSL, SST, and Transition SST

Models (p. )), or Shielded Detached Eddy Simulation (Including the SDES or SBES Model with BSL, SST,

and Transition SST Models (p. )).

Figure . : The Viscous Model Dialog Box Displaying the BSL k-ω Model

If you choose the shear-stress transport -

scale-resolving simulation options: Stress-Blended Eddy Simulation or Shielded Detached Eddy Simulation

(Including the SDES or SBES Model with BSL, SST, and Transition SST Models (p. )).

Figure . : The Viscous Model Dialog Box Displaying the SST k-ω Model

To enable the GEKO turbulence model, you must select the k-omega ( eqn) model on the Viscous

Model dialog box and then select GEKO in the k-omega Model group box.

If you intend to combine the GEKO model with a Reynolds Stress Model, you must first select one of

the following models:

Reynolds Stress Model based on BSL equation (Stress-BSL)

Wallin-Johansson Explicit Algebraic Reynolds Stress Model (WJ-BSL-EARSM, beta feature)

You can then enable the GEKO option in the Options group box of the Viscous Model dialog box.

In most cases, you would only tune the coefficients

and

.

. Optimize the coefficient

for the separation characteristics of wall boundary layers, which in most

applications has the strongest impact on performance.

. Adjust

to affect the mixing behavior of free shear flows (free mixing layers, etc. ).

For more details regarding these coefficients, see Generalized k-ω (GEKO) Model (p. ) and Generalized

k-ω  (GEKO) Model in the Fluent Theory Guide.

As these coefficients are both available through UDF, you can also adjust them differently in different

parts of the domain. The other two parameters can, in most cases, be left to their default settings.

By default, the full model is enabled and gives access to all model coefficients and the blending

function in the GEKO Options group box (Figure . : The Viscous Model Dialog Box with GEKO

Options for the Full Model  (p. )). For the wall distance free model option, only a subset of model

coefficients can be used (Figure . : The Viscous Model Dialog Box with GEKO Options for the Wall

Distance Free Version (p. )).

The corresponding text command to enable the GEKO turbulence model is

/define/models/viscous/kw-geko?

For combination with Reynolds stress models you must first enable the corresponding Reynolds Stress

Model and then use the TUI command.

/define/models/viscous/rsm-or-earsm-geko-option?

After GEKO is enabled, all model coefficients and the blending function are available in the submenu

geko-options:

/define/models/viscous/geko-options/wall-distance-free?

/define/models/viscous/geko-options/csep

/define/models/viscous/geko-options/cnw

/define/models/viscous/geko-options/cmix

/define/models/viscous/geko-options/cjet

/define/models/viscous/geko-options/blending-function

The auxiliary coefficients are also available as TUI commands.

/define/models/viscous/geko-options/creal

/define/models/viscous/geko-options/cnw_sub

/define/models/viscous/geko-options/cjet_aux

/define/models/viscous/geko-options/cbf_lam

/define/models/viscous/geko-options/cbf_tur

Furthermore, it is possible to reset these model parameters to default values by clicking GEKO Defaults

or the TUI command:

/define/models/viscous/geko-options/geko-defaults

Figure . : The Viscous Model Dialog Box with GEKO Options for the Full Model

Figure . : The Viscous Model Dialog Box with GEKO Options for the Wall Distance Free Version

If you choose the Transition -

model, it is not necessary to modify any of the model constants.

If you choose the Transition SST model (also known as the -

model), the following options are

roughness correlation (Transition SST and Rough Walls in the Theory Guide)

Setting Up the Transition SST Model

Stress-Blended Eddy Simulation (Including the SDES or SBES Model with BSL, SST, and Transition SST Mod-

els (p. )), or Shielded Detached Eddy Simulation (Including the SDES or SBES Model with BSL, SST, and

Transition SST Models (p. )).

Figure . : The Viscous Model Dialog Box for the Transition SST Model

You can customize your transition correlations, which are used in conjunction with the Transition SST

model. The user-defined functions that you can hook are:

transition length function (F_length).

critical momentum thickness Reynolds number (Re_thetac).

transition onset momentum thickness Reynolds number (Re_thetat).

For detailed information about the transition correlation UDFs, see DEFINE_TRANS UDFs in the Fluent

The Intermittency Transition model (also known as the  model) is available as an option for the following

turbulence models:

BSL -

model

SST -

model

Scale-Adaptive Simulation with BSL / SST

Detached Eddy Simulation with BSL / SST

BSL -

model

SST -

model

Shielded Detached Eddy Simulation (SDES) with BSL or SST

Stress-Blended Eddy Simulation (SBES) with BSL / SST

To apply it in combination with one of these turbulence models, you must enable the Intermittency

Transition Model option from the Options group box in the Viscous Model dialog box.

Figure . : The Intermittency Transition Model in Combination with the SST k-ω Model

After you have enabled the Intermittency Transition model, the additional option Include Crossflow

Transition will be available. This additional option allows you to include the effects of crossflow instability.

If you choose the RSM, the following submodels are available:

based Reynolds stress models:

– linear pressure-strain model (see Linear Pressure-Strain Model in the Theory Guide)

Setting Up the Reynolds Stress Model

– quadratic pressure-strain model (see Quadratic Pressure-Strain Model in the Theory Guide)

– Stress-Omega (see Stress-Omega Model in the Theory Guide)

– Stress-BSL (see Stress-BSL Model in the Theory Guide)

Figure . : The Viscous Model Dialog Box Displaying the Reynolds Stress Model Options

The following options are specific to the Reynolds-stress models based on the -equation:

wall boundary conditions for the Reynolds stresses from the  equation (Solving the k Equation to Obtain

Wall Boundary Conditions (p. )) for the linear and quadratic pressure-strain models

wall reflection effects on Reynolds stresses (Including the Wall Reflection Term (p. )) for the linear pressure-

strain model

near-wall treatments (see Near-Wall Treatments for Wall-Bounded Turbulent Flows in the Theory Guide):

– standard wall functions

– scalable wall functions

– non-equilibrium wall functions

– enhanced wall treatment (only for the linear pressure-strain model)

For the Reynolds stress models based on the

(Stress-Omega) and BSL-equation (Stress-BSL), a near-

wall treatment is automatically used to perform a blending between the viscous sublayer and the log-

arithmic region, and therefore near-wall treatment options are not shown. A low Re-number (LRN) mesh

is recommended for these models.

For Stress-Omega, you do have the option of selecting any or all of the following

options:

For both Stress-Omega and Stress-BSL, the following scale-resolving simulation option is available:

Scale-Adaptive Simulation (Setting Up Scale-Adaptive Simulation (SAS) Modeling (p. )).

Figure . : The Viscous Model Dialog Box Displaying the Stress-Omega Model Options

Other options that are available for both - and

based Reynolds stress models depending on your

case setup include:

Guide)

Note

The

based Reynolds stress models are not compatible with the Eulerian multiphase model.

Scale-Adaptive Simulation (SAS) modeling is an approach for the simulation of unsteady turbulent flows,

and can be applied in combination with most

based URANS turbulence models. To apply it in com-

bination with the SST -

turbulence model, you can simply select Scale-Adaptive Simulation (SAS)

from the Model list in the Viscous Model dialog box.

Figure . : Scale-Adaptive Simulation (SAS) in Combination with the SST Turbulence Model

You can also apply SAS in combination with the following

based URANS models: the Standard -

model, the BSL -

model, the Transition SST model, and the

based Reynolds stress models (RSM).

Simply select the appropriate Model and then enable the Scale-Adaptive Simulation (SAS) option in

the Scale-Resolving Simulation Options group box. For an example, see Figure . : Scale-Adaptive

Simulation (SAS) in Combination with the Transition SST Model (p. ).

Figure . : Scale-Adaptive Simulation (SAS) in Combination with the Transition SST Model

Note that for SAS modeling, the Bounded Central Differencing scheme (available in the Solution

Methods task page) is recommended for momentum discretization, and is the default setting.

Setting Up Scale-Adaptive Simulation (SAS) Modeling

When using the Detached Eddy Simulation (DES) model, the following underlying RANS turbulence

models can be used:

Spalart-Allmaras

Realizable -

SST -

BSL -

Transition SST

Note that for the DES model, the Bounded Central Differencing scheme (available in the Solution

... Setting Up DES with the Spalart-Allmaras Model

... Setting Up DES with the Realizable k-ε Model

... Setting Up DES with the SST k-ω Model

... Setting Up DES with the BSL k-ω Model

... Setting Up DES with the Transition SST Model

To set up a Detached Eddy Simulation with the Spalart-Allmaras model, select Detached Eddy Simu-

lation (DES) from the Model list in the Viscous Model dialog box and then select Spalart-Allmaras

from the RANS Model list.

ANSYS Fluent uses Equation . (in the Theory Guide) to compute the value of the length scale

for the Spalart-Allmaras model. By default, the empirical constant

is set to .. You can change

its value in the Cdes field under Model Constants. The following options are available for this model:

delayed DES (Delayed Detached Eddy Simulation (DDES) (p. ))

Figure . : The Viscous Model Dialog Box Displaying Options for DES with the Spalart-Allmaras

Model

Additionally, you can perform the following DES-specific function by using the /define/models/vis-

cous/detached-eddy-simulation? text command:

Modify only the length scales that appear in the destruction term in

equation (the default is to modify

all length scales within the

equation)

Setting Up the Detached Eddy Simulation Model

To set up a Detached Eddy Simulation with the Realizable -  model, select Detached Eddy Simulation

(DES) from the Model list in the Viscous Model dialog box and then select Realizable k-epsilon from

the RANS Model list.

The model-specific options for DES with the Realizable -  model are the following:

The model constant

is set to . for the Realizable -  model (see DES with the Realizable k-ε

Model in the Theory Guide). The enhanced wall treatment (EWT- ) is always enabled for DES with the

Realizable -  model (see Enhanced Wall Treatment ε-Equation (EWT-ε) in the Theory Guide).

Figure . : The Viscous Model Dialog Box Displaying Options for DES with the Realizable

k-ε Model

To set up a Detached Eddy Simulation with the SST -

model, select Detached Eddy Simulation

(DES) from the Model list in the Viscous Model dialog box and then select SST k-omega from the

RANS Model list.

The model-specific options that you can select for DES with the SST -

model are the following:

low-Re corrections -

option (Low-Re Corrections (p. ))

Shielding functions—F1, F2, DDES (Delayed DES) and IDDES (Improved Delayed DES)—are available when

the delayed DES option is enabled (Shielding Functions for the BSL / SST / Transition SST Detached Eddy

Simulation Model (p. ))

is set to . for the SST -

RANS model (see DES with the BSL or SST k-

ω Model in the Theory Guide).

Figure . : The Viscous Model Dialog Box Displaying Options for DES with the SST k-ω Model

To set up a Detached Eddy Simulation with the BSL -

model for a transient case, select k-omega

from the Model list in the Viscous Model dialog box, select BSL from the k-omega Model list, and

enable the Detached Eddy Simulation (DES) option in the Scale-Resolving Simulation Options

group box.

The model-specific options that you can select for DES with the BSL -

is set to . for the BSL -

Figure . : The Viscous Model Dialog Box Displaying Options for DES with the BSL k-ω Model

To set up a Detached Eddy Simulation with the Transition SST model for a transient case, select

Transition SST from the Model list in the Viscous Model dialog box and then enable the Detached

Eddy Simulation (DES) option in the Scale-Resolving Simulation Options group box.

For DES with the Transition SST model, you can choose to enable the Delayed DES option in the DES

Options group box (see Delayed Detached Eddy Simulation (DDES) (p. ) for details). When this option

is enabled you can make a selection from the Shielding Functions list, as described in Shielding

Functions for the BSL / SST / Transition SST Detached Eddy Simulation Model (p. ).

Figure . : The Viscous Model Dialog Box Displaying Options for DES with the Transition SST

Model

If you choose the LES model, the following subgrid-scale submodels are available (Subgrid-Scale Mod-

el (p. )):

Smagorinsky-Lilly

WALE

WMLES

WMLES S-Omega

Kinetic-Energy Transport

The default Subgrid-Scale Model for the LES model is the WALE model.

Figure . : The Viscous Model Dialog Box Displaying the Large Eddy Simulation Model Options

The LES options that are available for the Smagorinsky-Lilly submodel are

Setting Up the Large Eddy Simulation Model

Dynamic Stress

Dynamic Energy Flux (available only when the Dynamic Stress option is enabled)

Dynamic Scalar Flux (available only when the Dynamic Stress option is enabled)

The LES options that are available when the Kinetic-Energy Transport submodel is selected are Dy-

namic Energy Flux and Dynamic Scalar Flux.

The Dynamic Fvar option is available for all of the subgrid-scale submodels when Non-Premixed

Combustion or Partially Premixed Combustion is selected in the Species Model Dialog Box (p. ).

This option enables the dynamic mixture fraction variance model. See The Non-Premixed Model for LES

in the Theory Guide for details.

When using the LES model, you can enable the Werner-Wengle near-wall treatment through the following

text command: define/models/viscous/near-wall-treatment/werner-wengle-wall-

fn?. See LES Near-Wall Treatment in the Theory Guide for details.

It is also possible to modify the Model Constants, but this is not necessary for most applications. For

more information about the constants, see Spalart-Allmaras Model through Large Eddy Simulation (LES)

Model (in the Theory Guide). Note that C1-PS and C2-PS are the constants

and

in the linear

pressure-strain approximation of Equation . and Equation . (in the Theory Guide), and C1’-PS

and C2’-PS are the constants

and

in Equation . (in the Theory Guide). C1-SSG-PS, C1’-SSG-

PS, C2-SSG-PS, C3-SSG-PS, C3’-SSG-PS, C4-SSG-PS, and C5-SSG-PS are the constants

,

,

,

,

,

, and

in the quadratic pressure-strain approximation of Equation . (in the Theory Guide).

As described in Embedded Large Eddy Simulation (ELES) in the Theory Guide, the Embedded Large

Eddy Simulation model is used when modeling a smaller embedded LES zone within a larger RANS

computational domain. Recall that the interface between the upstream RANS zone and the LES zone

must be defined (by assigning the interface to a velocity fluctuation algorithm). In addition, the interface

between the LES zone and the downstream RANS zone must be considered.

This section describes how to set up the Embedded Large Eddy Simulation model.

. In the Viscous Model dialog box, enable any RANS model (for example,

,

), or you can select

DES, SAS, SDES, or SBES.The only RANS model not compatible with ELES is the Spalart-Allmaras

model, as a one-equation model cannot provide the required turbulent length scale to the interface

method.

If a RANS model is selected, the model is applied globally to the computational domain, however,

values for turbulence variables are frozen within the ELES region. The frozen state of the ELES

zone is used to determine the flow conditions (for - ,

, and so on) at the downstream LES-

RANS zone interface. Note that this approach requires a fairly well converged global RANS

solution to start with.

If DES, SAS, SDES, or SBES is used in the outer zone, these models are not frozen, but run in

the background in the ELES region, obtaining proper flow conditions (for - ,

, etc.) at the

downstream LES-RANS zone interface.

. For the specified fluid cell zone, enable LES Zone in the Fluid dialog box (Figure . : Specifying an

ELES Zone in the Fluid Dialog Box (p. )).This enables the Embedded LES tab in the Fluid dialog

box.

Note

When DES, SAS, SDES, or SBES is used for the global model, this and the next step

can, but need not, be skipped. (Remember the general limitations of DES in free,

box.

Note

wall-independent flows.) If you choose to skip these steps, then proceed with step

.

The ELES Zone option will only appear in the Fluid dialog box if you select the

Transient Solver. This must be done manually for RANS models.

. In the Embedded LES tab, you can then specify the Embedded Subgrid-Scale Model, and the Mo-

mentum Spatial Discretization.

For the Embedded Subgrid-Scale Model, the following subgrid-scale submodels are available

(Subgrid-Scale Model (p. )):

WALE

Dynamic Smagorinsky (which is the same as the LES model with Smagorinsky-Lilly selected

and the Dynamic Stress option enabled)

WMLES

The default Embedded-Subgrid Scale Model for the ELES model is the WALE model.

When the WALE model is selected, you can specify a value for Cwale to define

(see Wall-

Adapting Local Eddy-Viscosity (WALE) Model in the Theory Guide for details). Likewise, when

the Smagorinsky-Lilly model is selected, you can specify a value for Cs to define

(see

Smagorinsky-Lilly Model in the Theory Guide for details).

For the Momentum Spatial Discretization, the following options are available:

Bounded Central Differencing

Central Differencing

Setting Up the Embedded Large Eddy Simulation (ELES) Model

Figure . : Specifying an ELES Zone in the Fluid Dialog Box

. Select an appropriate interior interface and designate it as the RANS-LES interface, by right-clicking

the boundary zone name in the tree (under Setup/Boundary Conditions) and selecting rans-les-in-

terface in the Type sub-menu.

Figure . : Specifying the RANS/LES Interface

The RANS/LES Interface dialog box (Figure . : The RANS/LES Interface Dialog Box (p. ))

will open, allowing you to assign a Zone Name, as well as the Fluctuating Velocity Algorithm

and the Number Of Vortices. The options for the Fluctuating Velocity Algorithm are:

No Perturbations

Spectral Synthesizer

Vortex Method

For more information about these options, refer to Inlet Boundary Conditions for Scale Resolving

Simulations in the Theory Guide.

Note that the Number Of Vortices is the amount of vortices that the selected method distributes

randomly over the face zone and uses to generate turbulent fluctuations. The value should be

large enough to make sure there are no spots on the face zone that are unaffected by any

vortex. Large numbers may slightly increase the CPU effort, but will not impair the results.

Note

The minimum advised number of vortices is approximately a quarter of the

number of cell faces at the LES side of the interface.

Figure . : The RANS/LES Interface Dialog Box

If the RANS/LES interface is a non-conformal mesh interface, you can find the name of the in-

terface interior zone that you want to change into a rans-les-interface zone by using the List

button in the Mesh Interfaces Dialog Box (p. ).

Important

It is recommended that the RANS-LES interface be situated in a region where

there is no backflow.

For more information about the various options available for the turbulence models, see Spalart-Allmaras

Model through Large Eddy Simulation (LES) Model (in the Theory Guide). Instructions for activating

these options are provided here.

... Including the Viscous Heating Effects

... Including Turbulence Generation Due to Buoyancy

... Including the Curvature Correction for the Spalart-Allmaras and Two-Equation Turbulence Models

... Including the Compressibility Effects Option

... Including Production Limiters for Two-Equation Models

... Including the Intermittency Transition Model

...Vorticity- and Strain/Vorticity-Based Production

... Delayed Detached Eddy Simulation (DDES)

... Differential Viscosity Modification

... Swirl Modification

... Low-Re Corrections

... Shear Flow Corrections

...Turbulence Damping

... Including Pressure Gradient Effects

... Including Thermal Effects

... Including the Wall Reflection Term

... Solving the k Equation to Obtain Wall Boundary Conditions

... Quadratic Pressure-Strain Model

... Stress-Omega and Stress-BSL Models

... Subgrid-Scale Model

... Customizing the Turbulent Viscosity

... Customizing the Turbulent Prandtl and Schmidt Numbers

... Modeling Turbulence with Non-Newtonian Fluids

... Including Scale-Adaptive Simulation with ω-Based URANS Models

... Including Detached Eddy Simulation with the Transition SST Model

... Including the SDES or SBES Model with BSL, SST, and Transition SST Models

... Shielding Functions for the BSL / SST / Transition SST Detached Eddy Simulation Model

For information about including viscous heating effects in your model, see Inclusion of the Viscous

Dissipation Terms in the Theory Guide and Solving Heat Transfer Problems (p. ).

If you specify a nonzero gravity force (in the Operating Conditions Dialog Box (p. )), and you are

modeling a non-isothermal flow, the generation of turbulent kinetic energy due to buoyancy (

in

Equation .) is, by default, always included in the  equation. However, ANSYS Fluent does not, by

default, include the buoyancy effects on .

To include the buoyancy effects on , you must turn on the Full Buoyancy Effects option under Options

in the Viscous Model Dialog Box (p. ).

This option is available for all three -  models and for the -based RSM (that is, with the Linear

Pressure-Strain or Quadratic Pressure-Strain model selected).

... Including the Curvature Correction for the Spalart-Allmaras and

Two-Equation Turbulence Models

Eddy-viscosity models display an insensitivity to streamline curvature and system rotation, which play

a significant role in many turbulent flows of practical interest, as described in Curvature Correction for

the Spalart-Allmaras and Two-Equation Models in the Theory Guide. A modification to the turbulence

production term is available to sensitize the following standard eddy-viscosity models to the effects

of streamline curvature and system rotation:

Spalart-Allmaras one-equation model

Standard, RNG, and Realizable ( - ) models

Standard ( -

), BSL, SST, and Transition SST

Scale-Adaptive Simulation (SAS)

Setup Options for All Turbulence Modeling

Detached Eddy Simulation with BSL (DES-BSL), with SST (DES-SST), with Spalart-Allmaras (DES-SA),

and with Realizable ( - ) model (DES-rke).

Shielded Detached Eddy Simulation (SDES)

Stress-Blended Eddy Simulation (SBES)

Note that both the RNG and Realizable ( - ) turbulence models already have their own terms to include

rotational or swirl effects (see RNG Swirl Modification and Modeling the Turbulent Viscosity in the

Theory Guide for more information). The curvature correction option should therefore be used with

caution for these two models and is offered mainly for completeness for RNG and Realizable ( - ).

Enable the Curvature Correction option under Options in the Viscous Model Dialog Box (p. ).

You can specify a value for CCURV under Curvature Correction Options to influence the strength of

the curvature correction if needed for a specific flow. You have the option of specifying a constant or

via a UDF.

The Compressibility Effects option is available under Options in the Viscous Model Dialog Box (p. )

for most -based models,

based models, and Reynolds stress models when the compressible form

of the ideal gas law or the real-gas model is enabled. This option can improve the prediction of free

shear layers at high Mach numbers. See Model Enhancements (p. ) for recommendations on when

to use this option. For details about how this correction is implemented, see Effects of Compressibility

on Turbulence in the k-ε Models and Compressibility Effects in the Theory Guide.

A disadvantage of standard two-equation turbulence models is the excessive generation of the turbu-

lence energy,

, in the vicinity of stagnation points. In order to avoid the buildup of turbulent kinetic

energy in the stagnation regions, two formulations are available in order to limit the production term

in the turbulence kinetic energy equations:

Production Limiter (for details, see Equation . in the Fluent Theory Guide)

Production Kato-Launder (for details, see Equation . in the Fluent Theory Guide)

Both these formulations can be accessed under Options in the Viscous Model dialog box. The Pro-

duction Limiter model coefficient

is called the Production Limiter Clip Factor and has a default

value of . This value can be modified under Model Constants once the Production Limiter formu-

lation is enabled.

You can use the following text commands to set the formulations:

Production Limiter

/define/models/viscous/turbulence-expert/production-limiter? [yes]

Production Kato-Launder

/define/models/viscous/turbulence-expert/kato-launder-model? [yes]

The Production Limiter is available for the following turbulence models:

Detached Eddy Simulation with BSL (DES-BSL), with SST (DES-SST), and with Realizable ( - ) models (DES-

rke)

By default, this limiter is enabled for all turbulence models based on the

equation.

rke)

equation.

The Production Kato-Launder formulation for the production term is available for the following tur-

bulence models:

Standard, and RNG ( - ) models

Detached Eddy Simulation with BSL (DES-BSL) and with SST (DES-SST)

The Kato-Launder formulation is enabled by default for the Transition SST model only.

The Intermittency Transition model is available for the BSL -

model, SST -

model, Scale-Adaptive

Simulation with BSL / SST, Detached-Eddy Simulation with BSL / SST, Shielded Detached Eddy Simulation

(SDES) with BSL / SST, and Stress-Blended Eddy Simulation (SBES) with BSL / SST. It can be included

by enabling Intermittency Transition Model in the Options group box in the Viscous Model dialog

box with the appropriate turbulence model selected.

When the Intermittency Transition Model option is enabled, the additional option Include Crossflow

Transition is available. It allows you to include the effects of crossflow instability.

For details about the Intermittency Transition model, see Intermittency Transition Model in the Theory

Guide.

For the Spalart-Allmaras model, you can choose either Vorticity-Based Production or Strain/Vorticity-

Based Production under Spalart-Allmaras Production in the Viscous Model Dialog Box (p. ). If

you choose Vorticity-Based Production, ANSYS Fluent will compute the value of the deformation

tensor  using Equation . (in the Theory Guide); if you choose Strain/Vorticity-Based Production,

it uses Equation . (in the Theory Guide).

(These options will not appear unless you have enabled the Spalart-Allmaras model.)

The Delayed DES option is recommended when using the DES model. This option preserves the RANS

model throughout the boundary layer. For more information, see Detached Eddy Simulation (DES) in

the Theory Guide.

The RNG turbulence model in ANSYS Fluent has an option of using a differential formula for the effective

viscosity

(Equation . in the Theory Guide) to account for the low-Reynolds-number effects. To

enable this option, the Differential Viscosity Model option under RNG Options in the Viscous Model

Dialog Box (p. ) must be enabled.

Important

This option appears when you have enabled the RNG -  model.

After you have chosen the RNG model, the swirl modification takes effect, by default, for all three-di-

mensional flows and axisymmetric flows with swirl. The default swirl constant (

in Equation . in

the Theory Guide) is set to ., which works well for weakly to moderately swirling flows. However,

for strongly swirling flows, you may need to use a larger swirl constant.

To change the value of the swirl constant, you must first enable the Swirl Dominated Flow option

under RNG Options in the Viscous Model Dialog Box (p. ).

Important

Important

This option will not appear unless you have enabled the RNG -  model.

If any of the -

models or the Stress-Omega RSM is used, you may enable a low-Reynolds-number

correction to the turbulent viscosity by enabling the Low-Re Corrections option under k-omega

Options in the Viscous Model dialog box. By default, this option is not enabled, and the damping

coefficient (

in Equation . in the Theory Guide) is equal to .

In the standard -

model and the Stress-Omega RSM, you also have the option of including corrections

to improve the accuracy in predicting free shear flows. The Shear Flow Corrections option under the

k-omega Options is enabled by default in the Viscous Model dialog box, as these corrections are

included in the standard -

model  [] (p. ). When this option is enabled, ANSYS Fluent will

calculate

using Equation . (in the Theory Guide) and

using Equation . (in the Theory

Guide). If this option is disabled,

and

will be set equal to .

For cases that use the VOF or Mixture multiphase models, or the Eulerian multiphase model with the

Multi-Fluid VOF option selected, you can enable Turbulence Damping (in the k-omega Options group

box). This option is required for better resolution of velocity gradients in the vicinity of fluid-fluid in-

terface. After enabling Turbulence Damping, you can specify the Damping Factor, which by default

is set to . For a theoretical discussion about turbulence damping, refer to Turbulence Damping in

Note

Note

Incorporation of turbulence damping is recommended only for sharp and sharp/dispersed

interface modeling types.

If the enhanced wall treatment is used, you may include the effects of pressure gradients by enabling

the Pressure Gradient Effects option under the Enhanced Wall Treatment Options. When this option

is enabled, ANSYS Fluent will include the coefficient  in Equation . (in the Theory Guide).

If the enhanced wall treatment is used, you may include thermal effects by enabling the Thermal Effects

option under Enhanced Wall Treatment Options. When this option is enabled, ANSYS Fluent will in-

clude the coefficient  in Equation . (in the Theory Guide).

will also be included in Equation .

when the Thermal Effects option is enabled if the ideal gas law is selected for the fluid density in the

If the RSM is used with the default model for linear pressure-strain, ANSYS Fluent will, by default, include

the wall-reflection effects in the pressure-strain term. That is, ANSYS Fluent will calculate

using

Equation . (in the Theory Guide) and include it in Equation . (in the Theory Guide). For the

quadratic pressure-strain model, Stress-Omega model, and Stress-BSL model, the wall-reflection effects

are not required and are not included.

Important

The empirical constants and the function  used in the calculation of

are calibrated

for simple canonical flows such as channel flows and flat-plate boundary layers involving a

Important

single wall. If the flow involves multiple walls and the wall has significant curvature (for

example, an axisymmetric pipe or curvilinear duct), the inclusion of the wall-reflection term

in Equation . (in the Theory Guide) may not improve the accuracy of the RSM predictions.

In such cases, you can disable the wall-reflection effects by turning off the Wall Reflection

Effects under Reynolds-Stress Options in the Viscous Model Dialog Box (p. ).

For the -based Reynolds stress models, by default ANSYS Fluent uses the explicit setting of boundary

conditions for the Reynolds stresses near the walls, with the values computed with Equation . (in

the Theory Guide). The turbulent kinetic energy,

, is calculated by solving the  equation obtained

by summing Equation . (in the Theory Guide) for normal stresses. To disable this option and use

the wall boundary conditions given in Equation . (in the Theory Guide), turn off the Wall BC from

k Equation under the Reynolds-Stress Options in the Viscous Model dialog box.

Important

This option will not appear unless you have enabled the Reynolds Stress model.

To use the quadratic pressure-strain model described in Quadratic Pressure-Strain Model (in the Theory

Guide), enable the Quadratic Pressure-Strain Model option under Reynolds-Stress Options in the

Viscous Model Dialog Box (p. ). (This option will not appear unless you have enabled the RSM.) The

following options are not available when the Quadratic Pressure-Strain Model is enabled:

Wall Reflection Effects under Reynolds-Stress Options

Enhanced Wall Treatment under Near-Wall Treatment

To use the Stress-Omega model (described in Stress-Omega Model) or the Stress-BSL model (described

in Stress-BSL Model), select Stress-Omega or Stress-BSL, respectively, from the Reynolds-Stress

Model list in the Viscous Model Dialog Box (p. ). (These options will not appear unless you have

enabled the RSM.) The following options are not available when the Stress-Omega or the Stress-BSL

model is selected:

Wall BC from k Equation under Reynolds-Stress Options

Standard Wall Functions under Near-Wall Treatment

Scalable Wall Functions under Near-Wall Treatment

Non-Equilibrium Wall Functions under Near-Wall Treatment

Instead, the following options are available:

Low-Re Corrections under k-omega Options (for Stress-Omega only)

Shear Flow Corrections under k-omega Options (for Stress-Omega only)

Scale-Adaptive Simulation (SAS) under Scale-Resolving Simulation Options

If you have selected the Large Eddy Simulation model, you will be able to choose one of the subgrid-

scale models described in Subgrid-Scale Models (in the Theory Guide). You can choose from the

Smagorinsky-Lilly, WALE, WMLES, WMLES S-Omega, or Kinetic-Energy Transport subgrid-scale

models. Note that Dynamic Stress is an option available with the Smagorinsky-Lilly model (and when

it is enabled, this model is referred to as the “dynamic Smagorinsky” model), while the Kinetic-Energy

Transport model is always run as a dynamic model. The Dynamic Fvar option is available for all of

the subgrid-scale models when Non-Premixed Combustion or Partially Premixed Combustion is

selected in the Species Model Dialog Box (p. ).

Important

These options will not appear unless you have enabled the LES model.

If you are using the Spalart-Allmaras,

,

, DES, or LES models, a UDF can be used to customize

the turbulent viscosity. This option will enable you to modify

in the case of the Spalart-Allmaras,

, and -

models, and incorporate completely new subgrid models in the case of the LES model.

SBES with BSL / SST allows the usage of a UDF in order to provide a custom formulation for

in the

RANS region, but not for the subgrid model in the LES region. More information about UDFs can be

found in the Fluent Customization Manual.

In the Viscous Model Dialog Box (p. ), under User-Defined Functions, select the appropriate user-

defined function in the Turbulent Viscosity drop-down list. For the LES model, select the appropriate

UDF in the Subgrid-Scale Turbulent Viscosity drop-down list.

You can use UDFs to customize the turbulent Prandtl and Schmidt numbers. For the standard and

realizable -  models and the standard -

model, your UDF can calculate the TKE Prandtl number

(

) and either the TDR or SDR Prandtl number (

or

), depending on whether you are using the

or -

model. All turbulence models allow you to use UDFs for the turbulent Prandtl number at

the wall (

in Equation . in the Theory Guide), and all turbulent models except for the RNG -

model allow you to use UDFs for the turbulent Prandtl number for energy (

in, for example, Equa-

tion . or Equation . in the Theory Guide), as well as the turbulent Schmidt number (

, in

Equation . in the Theory Guide) if species transport has been enabled. Note that UDFs cannot be

used for the turbulent Prandtl number for energy or the turbulent Schmidt number if you have enabled

Dynamic Energy Flux or Dynamic Scalar Flux, respectively, as part of the LES model. More information

about UDFs can be found in the Fluent Customization Manual.

In the Viscous Model Dialog Box (p. ), under User-Defined Functions, select the appropriate UDF

from the drop-down lists in the Prandtl Numbers or Prandtl and Schmidt Numbers group box. The

options will depend on the turbulence model you have selected (as noted previously), and include:

TKE Prandtl Number, TDR Prandtl Number, SDR Prandtl Number, Energy Prandtl Number, Wall

Prandtl Number, and Turbulent Schmidt Number. Note that the availability of these drop-down lists

can be affected by your settings for the energy equation and the multiphase and combustion models.

If the turbulent flow involves non-Newtonian fluids, you can use the define/models/ viscous/tur-

bulence-expert/turb-non-newtonian? text command to enable the selection of non-Newto-

nian options for the material viscosity. See Viscosity for Non-Newtonian Fluids (p. ) for details about

these options.

You have the option of including Scale-Adaptive Simulation (SAS) with most

based URANS models.

For details about SAS and how to include it, see Scale-Adaptive Simulation (SAS) (p. ) and Setting

Up Scale-Adaptive Simulation (SAS) Modeling (p. ), respectively.

... Including Detached Eddy Simulation with the Transition SST

Model

You have the option of including Detached Eddy Simulation (DES) with the Transition SST model. For

details about DES and how to include it, see Detached Eddy Simulation (DES) (p. ) and Setting Up

DES with the Transition SST Model (p. ), respectively.

... Including the SDES or SBES Model with BSL, SST, and Transition

SST Models

To enable a hybrid RANS-LES model with an improved shielding function compared to DDES / IDDES,

you can enable the Stress Blending (SBES) / Shielded DES option in the Scale-Resolving Simulation

Options group box of the Viscous Model dialog box. This option is available for 3D transient cases

when you have selected one of the following models (see Figure . : The Viscous Model Dialog Box

with the SBES Options (p. )):

Generalized -

(GEKO) model

Baseline (BSL) -

model

Shear-Stress Transport (SST) -

model

You can then select one of the following from the Hybrid Model list:

model

model

SDES to apply only a shielding function (Shielded Detached Eddy Simulation (SDES) in the Fluent Theory

Guide)

SBES to apply a shielding function with stress blending (Stress-Blended Eddy Simulation (SBES) in the Fluent

Theory Guide)

SBES with User-Defined Function to define your own blending function zonally for cases where the division

between RANS and LES is clear from the geometry and the flow physics ( DEFINE_SBES_BF in the Fluent

Customization Manual)

If you select SBES or SBES with User-Defined Function for the Hybrid Model, you can also select

one of the following subgrid-scale (LES) models:

Smagorinsky-Lilly model

Dynamic Smagorinsky-Lilly model

Wall-Adapting Local Eddy-Viscosity (WALE) model

Algebraic Wall-Modeled LES -  (WMLES S-Omega) model

The WALE model is recommended, as it provides the lowest eddy viscosity in 2D flow regions and

thereby allows the flow to quickly develop 3D turbulence structures in separating shear layers. The

combination of SBES with the WMLES S-Omega formulation is likely not a useful combination, as the

SBES-WALE model combination can by itself act in a WMLES mode.

If you select SBES or SBES with User-Defined Function for the Hybrid Model, you can also specify

an integer value (between  and ) for Update Interval k-omega, which determines how often the

and

equations are computed during a run.

In many cases, the global time step required for the LES portion of the calculation is unnecessarily fine

for the RANS portion. For this reason, it is not required that the -

part of the SBES model is updated

after every time step. Reducing the frequency at which the -

equations are solved by specifying an

update interval can positively impact the solution time, with minimal impact on the solution or con-

vergence. An optimal value for the parameter is . Note that the momentum equations as well as the

LES eddy-viscosity portion of the SBES model are updated at every time step. The parameter only reduces

the number of updates of the  and

equations, as well as that of the blending function.

For example, if you specify an update interval of , the solver would update the -

portion every

5th timestep, while still updating the LES eddy viscosity portion every timestep.

Note

The Update Interval k-omega functionality has the following limitations:

Not compatible with multiphase flow.

Not compatible with adaptive time-stepping.

The time scheme for the  and

equations are automatically set to first order in cases of variable

density flow or moving meshes.The time scheme for other equations is not affected by this.

Figure . : The Viscous Model Dialog Box with the SBES Options

Note

For the SDES and SBES models, the Bounded Central Differencing scheme (available in

the Solution Methods task page) is recommended for momentum discretization, and is

the default setting.

... Shielding Functions for the BSL / SST / Transition SST Detached

Eddy Simulation Model

For the DES model with the BSL -

model, or the Transition SST model, the shielding

(or blending) functions F1 and F2 are defined in Equation . and Equation . in the Theory

Guide, respectively. Note that the F2 function is more conservative than the F1 function. In addition,

the shielding functions DDES (Delayed DES) and IDDES (Improved Delayed DES), are described in DES

with the BSL or SST k-ω Model and Improved Delayed Detached Eddy Simulation (IDDES) in the Theory

Guide. DDES is recommended and is used as the default.

...Wall Roughness Effects

...The Spalart-Allmaras Model

... k-ε Models and k-ω Models

... Reynolds Stress Model

... Large Eddy Simulation Model

You may want to include the effects of the wall roughness on selected wall boundaries as part of your

turbulent simulation. In such cases, you can specify the roughness parameters (roughness height and

roughness constant) in the dialog boxes of the corresponding wall boundaries (see Setting the

Roughness Parameters (p. )).

Note

model

model

When you are modeling turbulent flows in ANSYS Fluent using the Spalart-Allmaras model, you must

provide the boundary conditions for  in addition to other mean solution variables. The boundary

conditions for  at the walls are internally taken care of by ANSYS Fluent, which obviates the need for

your inputs. The boundary condition input for , which you must enter in ANSYS Fluent, is the one at

inlet boundaries (for example, velocity inlets, pressure inlets). In many situations, it is important to

specify correct or realistic boundary conditions at the inlets, because the inlet turbulence can significantly

affect the downstream flow.

When you are modeling turbulent flows in ANSYS Fluent using one of the -  models or one of the

models, you must provide the boundary conditions for  and  (or  and

) in addition to other

mean solution variables. The boundary conditions for  and  (or  and

) at the walls are internally

taken care of by ANSYS Fluent, which obviates the need for your inputs. The boundary condition inputs

for  and  (or  and

), which you must enter in ANSYS Fluent, are the ones at inlet boundaries (for

example, velocity inlets, pressure inlets). In many situations, it is important to specify correct or realistic

boundary conditions at the inlets, because the inlet turbulence can significantly affect the downstream

flow.

See Determining Turbulence Parameters (p. ) for details about specifying the boundary conditions

) at the inlets.

flow.

Additionally, you can control whether or not to set the turbulent viscosity to zero within a laminar

zone. If the fluid zone in question is laminar, the text command define/ boundary-condi-

tions/fluid will contain an option called Set Turbulent Viscosity to zero within

laminar zone?. By setting this option to yes, ANSYS Fluent will set both the production term in

the turbulence transport equation and

to zero. In contrast, when the Laminar Zone option is enabled

in a Fluid cell zone condition dialog box, only the production term is set to zero. See Specifying a

Laminar Zone (p. ) for details about laminar zones.

Important

Note that the laminar zone feature is also available for the Spalart-Allmaras and Reynolds

stress models.

The specification of turbulent boundary conditions for the RSM is the same as for the other turbulence

models for all boundaries except at boundaries where flow enters the domain. Additional input

methods are available for these boundaries and are described here.

When you choose to use the RSM, the default inlet boundary condition inputs required are identical

to those required when the -  model is active. You can input the turbulence quantities using any of

the turbulence specification methods described in Determining Turbulence Parameters (p. ). ANSYS

Defining Turbulence Boundary Conditions

Fluent then uses the specified turbulence quantities to derive the Reynolds stresses at the inlet from

the assumption of isotropy of turbulence:

(.)

(.)

where

is the normal Reynolds stress component in each direction. The boundary condition for

(.)

(.)

where

is determined in the same manner as for the -  turbulence models (see Determining Turbulence

Parameters (p. )). To use this method, you will select K or Turbulent Intensity as the Reynolds-

Stress Specification Method in the appropriate boundary condition dialog box.

Alternately, you can directly specify the Reynolds stresses by selecting the Reynolds-Stress Components

as the Reynolds-Stress Specification Method in the boundary condition dialog box. When this option

is selected, you should input the Reynolds stresses directly.

You can set the Reynolds stresses by using constant values, profile functions of coordinates (see Pro-

files (p. )), or user-defined functions (in the Fluent Customization Manual).

Figure . : Specifying Inlet Boundary Conditions for the Reynolds Stresses

It is possible to specify the magnitude of random fluctuations of the velocity components at an inlet

only if the velocity inlet boundary condition is selected. In this case, you must specify a Turbulence

Intensity that determines the magnitude of the random perturbations on individual mean velocity

components as described in Inlet Boundary Conditions for Scale Resolving Simulations (in the Theory

Guide). For all boundary types other than velocity inlets, the boundary conditions for LES remain the

same as for laminar flows.

For flows using one of the -  models, one of the -

models, or the RSM, the converged solutions or

(for unsteady calculations) the solutions after a sufficiently long time has elapsed should be independent

of the initial values for  and  (or  and

). For better convergence, however, it is beneficial to use a

reasonable initial guess for  and  (or  and

).

In general, it is recommended that you start from a suitable state of turbulence. When using a

in-

sensitive wall treatment, it is critically important to specify suitable turbulence fields. Guidelines are

provided below:

If you were able to specify reasonable boundary conditions at the inlet, it may be a good idea to compute

the initial values for  and  (or  and

) in the whole domain from these boundary values. See Initializing

the Solution (p. ) for details.

For more complex flows (for example, flows with multiple inlets with different conditions) it may be better

to specify the initial values in terms of Turbulent Intensity and Turbulent Viscosity Ratio, which can both

be specified at the inlet(s). For Turbulent Intensity,

, typical values lie in the range of -%. For Turbulent

Viscosity Ratio, typical values lie in the range of -.

– The value of  can then be computed from the Turbulent Intensity and the characteristic mean velocity

magnitude of your problem (note that in the following calculation for ,

must be given as a fraction):

(.)

– You should specify an initial guess for  so that the resulting eddy viscosity (

) is sufficiently large in

comparison to the molecular viscosity. Suitable levels of turbulent viscosity are typically in the range of

times larger than the molecular viscosity. From this, you can compute :

(.)

where

is the Turbulent Viscosity Ratio which can be prescribed at the inlet and then used for

the domain initialization.

– Similarly, for the specific dissipation rate,

:

(.)

Note that, for the RSM, Reynolds stresses are initialized automatically using Equation . (p. ) and

Compared to laminar flows, simulations of turbulent flows are more challenging in many ways. For the

Reynolds-averaged approach, additional equations are solved for the turbulence quantities. Since the

equations for mean quantities and the turbulent quantities (

,

, ,

, or the Reynolds stresses) are

strongly coupled in a highly nonlinear fashion, it takes more computational effort to obtain a converged

turbulent solution than to obtain a converged laminar solution. The LES model, while embodying a

simpler, algebraic model for the subgrid-scale viscosity, requires a transient solution on a very fine mesh.

The fidelity of the results for turbulent flows is largely determined by the turbulence model being used.

Here are some guidelines that can enhance the quality of your turbulent flow simulations.

... Mesh Generation

... Accuracy

... Convergence

... RSM-Specific Solution Strategies

... LES-Specific Solution Strategies

The following are suggestions to follow when generating the mesh for use in your turbulent flow

simulation:

First imagine the flow under consideration, then identify the main flow features expected in the flow using

your physical intuition or any data for a similar flow situation. Generate a mesh that can resolve the major

features that you expect.

If the flow is wall-bounded and the wall is expected to affect the flow significantly, you should take addi-

tional care when generating the mesh. See Grid Resolution for RANS Models (p. ) and Wall Boundary

Layers (p. ) for guidelines.

The suggestions below are provided to help you obtain better accuracy in your results:

Use the turbulence model that is better suited for the salient features you expect to see in the flow (see

Choosing a Turbulence Model (p. )).

Because the mean quantities have larger gradients in turbulent flows than in laminar flows, it is recommen-

ded that you use high-order schemes for the convection terms.This is especially true if you employ a trian-

gular or tetrahedral mesh. Note that excessive numerical diffusion adversely affects the solution accuracy,

even with the most elaborate turbulence model.

In some flow situations involving inlet boundaries, the flow downstream of the inlet is dictated by the

boundary conditions at the inlet. In such cases, you should exercise care to make sure that reasonably

realistic boundary values are specified.

The suggestions below are provided to help you enhance convergence for turbulent flow calculations:

Starting with excessively crude initial guesses for mean and turbulence quantities may cause the solution

to diverge. A safe approach is to start your calculation using conservative (small) under-relaxation parameters

and (for the density-based solvers) a conservative Courant number, and increase them gradually as the it-

erations proceed and the solution begins to settle down.

It is also helpful for faster convergence to start with reasonable initial guesses for the  and  (or  and

)

fields. Particularly when a

insensitive wall treatment is used, it is important to start with a sufficiently

developed turbulence field, as recommended in Providing an Initial Guess for k and ε (or k and ω) (p. ),

to avoid the need for an excessive number of iterations to develop the turbulence field.

Solution Strategies for Turbulent Flow Simulations

When you are using the RNG -  model, an approach that might help you achieve better convergence is

to obtain a solution with the standard -  model before switching to the RNG model. Due to the additional

nonlinearities in the RNG model, lower under-relaxation factors and (for the density-based solvers) a lower

Courant number might also be necessary.

Note that when you use the enhanced wall treatment (EWT- ), you may sometimes find during the

calculation that the residual for  is reported to be zero. This happens when your flow is such that

is less than  in the entire flow domain, and  is obtained from the algebraic formula (Equa-

tion . in the Theory Guide) instead of from its transport equation.

Using the RSM creates a high degree of coupling between the momentum equations and the turbulent

stresses in the flow, and therefore the calculation can be more prone to stability and convergence

difficulties than with the -  models. When you use the RSM, therefore, you may need to adopt special

solution strategies in order to obtain a converged solution. The following strategies are generally re-

commended:

Begin the calculations using the standard -  model.Turn on the RSM and use the -  solution data as a

starting point for the RSM calculation.

Use low under-relaxation factors (. to .) and (for the density-based solvers) a low Courant number for

highly swirling flows or highly complex flows. In these cases, you may need to reduce the under-relaxation

factors both for the velocities and for all of the stresses.

Instructions for setting these solution parameters are provided below. If you are applying the RSM to

prediction of a highly swirling flow, you will want to consider the solution strategies discussed in

Swirling and Rotating Flows (p. ) as well.

.... Under-Relaxation of the Reynolds Stresses

ANSYS Fluent applies under-relaxation to the Reynolds stresses. You can set under-relaxation factors

using the Solution Controls Task Page (p. ).

Solution →

Controls

The default settings of . are recommended for most cases. You may be able to increase these settings

and speed up the convergence when the RSM solution begins to converge.

In some situations, when poor convergence is observed one might facilitate the convergence rates

by modifying some of the under-relaxation values whilst leaving the others unchanged. This might

be a more successful approach than the simple scaling of all under-relaxation values.

.... Disabling Calculation Updates of the Reynolds Stresses

In some instances, you may want to let the current Reynolds stress field remain fixed, skipping the

solution of the Reynolds transport equations while solving the other transport equations. You can

enable/disable all Reynolds stress equations in the Equations dialog box.

Solution → Controls

Equations...

.... Residual Reporting for the RSM

When you use the RSM for turbulence, ANSYS Fluent reports the equation residuals for the individual

Reynolds stress transport equations. You can apply the usual convergence criteria to the Reynolds

stress residuals: normalized residuals in the range of

usually indicate a practically-converged

solution. However, you may need to apply tighter convergence criteria (below

) to ensure full

Large eddy simulation involves running a transient solution from some initial condition, on an appro-

priately fine mesh, using an appropriate time step size. The solution must be run long enough to become

independent of the initial condition and to enable the statistics of the flow field to be determined.

The following are suggestions to follow when running a large eddy simulation:

. Start by running a steady-state flow simulation using a Reynolds-averaged turbulence model such as

standard - ,

, or even RSM. Run until the flow field is reasonably converged and then use the

solve/initialize/init-turb-vel-fluctuations text command to generate the instantaneous

velocity field out of the steady-state RANS results.This command must be executed before LES is enabled.

This option is available for all RANS-based models and it will create a much more realistic initial field for

the LES run. Additionally, it will help in reducing the time needed for the LES simulation to reach a statist-

ically stable mode.This step is optional.

. When you enable LES, ANSYS Fluent will automatically turn on the unsteady solver option and

choose the second-order implicit formulation. You will need to set the appropriate time step size

and all the needed solution parameters. (See User Inputs for Time-Dependent Problems (p. ) for

guidelines on setting solution parameters for transient calculations in general.) For the pressure-

based solver, the bounded central differencing spatial discretization scheme will be automatically

selected for momentum equations; both the bounded central-differencing and pure central-differ-

encing schemes are available for all equations when running LES simulations. For the density-based

solver, the bounded central differencing scheme can be used for the flow equations, though it is

not selected by default.

. Run LES until the flow becomes statistically steady.The best way to see if the flow is fully developed and

statistically steady is to monitor forces and solution variables (for example, velocity components or pressure)

at selected locations in the flow.

. Zero out the initial statistics using the solve/initialize/init-flow-statistics text

command. Before you restart the solution, enable Data Sampling for Time Statistics in the Run

Calculation Task Page (p. ), as described in User Inputs for Time-Dependent Problems (p. ).

With this option enabled, ANSYS Fluent will gather data for time statistics while performing a large

eddy simulation. You can set the Sampling Interval such that Data Sampling for Time Statistics

can be performed at the specified frequency. When Data Sampling for Time Statistics is enabled,

the statistics collected at each sampling interval can be postprocessed and you can then view both

the mean and the root-mean-square-error (RMSE) values in ANSYS Fluent. The Sampled Time displays

the time period over which data has been sampled for the postprocessing of the mean and RMSE

values. As long as the time step size has been constant, dividing this by the time step size yields

the number of data sets that have been collected. If the time step size is varied, every contribution

of data sets sampled is automatically weighted by the current time step size.

. Continue until you get statistically stable data.The duration of the simulation can be determined before-

hand by estimating the mean flow residence time in the solution domain (

, where  is the character-

istic length of the solution domain and

is a characteristic mean flow velocity).The simulation should

be run for at least a few mean flow residence times.

Instructions for setting the solution parameters for LES are provided below.

....Temporal Discretization

ANSYS Fluent provides both first-order and second-order temporal discretizations. For LES, the second-

order discretization is recommended.

Solution →

Methods

Overly diffusive schemes such as the first-order upwind scheme should be avoided, because they

may unduly damp out the energy of the resolved eddies. The central-differencing based schemes are

recommended for all equations when you use the LES model. ANSYS Fluent provides two central-

differencing based schemes: pure central-differencing and bounded central-differencing. The bounded

scheme is the default option for momentum discretization when you select LES, SAS, DES, SDES, or

SBES.

Solution →

Methods

ANSYS Fluent provides postprocessing options for displaying, plotting, and reporting various turbulence

quantities, which include the main solution variables and other auxiliary quantities.

Turbulence quantities that can be reported for the Spalart-Allmaras model are as follows:

Wall Yplus

Curvature Correction Function fr (only when the curvature correction is enabled)

Turbulence quantities that can be reported for the DES model in combination with the Spalart-All-

maras model are as follows:

all of the quantities available for the Spalart-Allmaras model

Note

Note

For a Detached Eddy Simulation with the Spalart-Allmaras model, the DES TKE Dissipation

Multiplier represents the function

in Equation ..

Turbulence quantities that can be reported for the -  models are as follows:

Wall Ystar

Wall Yplus

Turbulent Reynolds Number (Re_y) (only when the enhanced wall treatment is used for the near-wall

treatment)

Turbulence quantities that can be reported for the DES model in combination with the Realizable -

model are as follows:

all of the quantities available for the Realizable -  model

Postprocessing for Turbulent Flows

Note

For a Detached Eddy Simulation with the Realizable -  model, the DES TKE Dissipation

Turbulence quantities that can be reported for the -

models are as follows:

Wall Ystar

Wall Yplus

Wall Ystar

Wall Yplus

Turbulence quantities that can be reported for the Standard and BSL -

model in combination with

the SAS model are as follows:

all of the quantities available for the -

model

Turbulence quantities that can be reported for the BSL or SST -

model in combination with the DES

models

Note

For a Detached Eddy Simulation with BSL / SST, DES TKE Dissipation Multiplier represents

the function

in Equation . and

in Equation ., depending on the specified

model. Within the DES concept, the DES TKE Dissipation Multiplier increases the destruction

term in the transport equation for the turbulence kinetic energy in LES regions (

).

This increase in destruction terms reduces the eddy viscosity in LES regions.

model in combination with the

Shielded Detached Eddy Simulation (SDES) model or the Stress-Blended Eddy Simulation (SBES) model

models

Turbulence quantities that can be reported for the transition -

Wall Ystar

Wall Yplus

Turbulence quantities that can be reported for the Transition SST model are as follows:

Wall Ystar

Wall Yplus

Turbulence quantities that can be reported for the Transition SST model in combination with the SAS

all of the quantities available for the Transition SST model

Turbulence quantities that can be reported for the Transition SST model in combination with the DES

Note

For the Transition SST model in combination with the DES model, DES TKE Dissipation

in Equation . de-

Note

pending on the specified model. Within the DES concept, the DES TKE Dissipation Multiplier

increases the destruction term in the transport equation for the turbulence kinetic energy

in LES regions (

). This increase in destruction terms reduces the eddy viscosity in LES

regions.

Turbulence quantities that can be reported for the Transition SST model in combination with the

Turbulence quantities that can be reported for the RSM are as follows:

UU Reynolds Stress

VV Reynolds Stress

WW Reynolds Stress

UV Reynolds Stress

VW Reynolds Stress

UW Reynolds Stress

Specific Dissipation Rate (Omega) (

based Reynolds stress models only)

Wall Ystar

Wall Yplus

Turbulent Reynolds Number (Re_y) ( -based Reynolds stress models only)

Turbulence quantities that can be reported for the

based Reynolds stress models in combination

with the SAS model are as follows:

all of the quantities available for the RSM model

Turbulence quantities that can be reported for the SAS model in combination with the SST -

model

Wall Yplus

Wall Ystar

Turbulence quantities that can be reported for the LES model are as follows:

Turbulence Kinetic Energy

Turbulence Intensity

Subgrid Dynamic Sc of Species

Wall Ystar

Wall Yplus

Additional turbulence quantities can be reported for the Embedded LES (ELES) model.

Note

Within the Embedded LES zone, the modeled eddy viscosity is determined by an algebraic

subgrid-scale eddy viscosity model. The global turbulence model is either frozen or, if it is

either SAS, DES, SDES, or SBES with an underlying two-equation RANS model, runs in a

"passive mode", that is without affecting the momentum equations.

Hence, most turbulence postprocessing in the Embedded LES zone refers to the frozen or

"passive" global turbulence model. Special care is necessary with the modeled eddy viscosity,

because there are two to consider: one from the frozen / passive global turbulence model;

and one from the "local" algebraic subgrid-scale model that is running within the Embedded

LES zone and actually affects the momentum equations.

Some postprocessing quantities refer to a "passive" global turbulence model or are zero if the global model

cannot run in "passive" mode and therefore is frozen in the Embedded LES zone.

– Turbulent Viscosity

– Turbulent Viscosity Ratio

In the Embedded LES zone, the subgrid-scale eddy viscosity from the local algebraic model, which actually

affects the momentum equations, is displayed as:

– LES Subgrid Turbulent Viscosity

The following quantities are specific to the Dynamic LES subgrid-scale eddy viscosity models.They are

available in Embedded LES zones if the Dynamic Smagorinsky model is used in any Embedded LES zone;

they are also available for global LES when the Smagorinsky-Lilly subgrid-scale model is selected with the

Dynamic Stress option enabled or when the Kinetic-Energy Transport subgrid-scale model is selected:

– Subgrid Test-Filter Length

– Subgrid Dynamic Viscosity Const

– Subtest Kinetic Energy

All of these variables can be found in the Turbulence... category of the variable selection drop-down

list that appears in postprocessing dialog boxes. See Field Function Definitions (p. ) for their definitions.

... Custom Field Functions for Turbulence

... Postprocessing Turbulent Flow Statistics

...Troubleshooting

In addition to the quantities listed in Postprocessing for Turbulent Flows (p. ), above, you can define

your own turbulence quantities using the Custom Field Function Calculator Dialog Box (p. ).

User-Defineed → Field Functions → Custom...

The following functions may be useful:

the ratio of production of  to its dissipation (

)

the ratio of the mean flow to turbulent time scale,  (

)

the Reynolds stresses derived from the Boussinesq formula (for example,

)

As described in Large Eddy Simulation (LES) Model (in the Theory Guide), LES involves the solution of

a transient flow field, but it is the mean flow quantities that are of interest from an engineering

standpoint.

For all other turbulent flow, if Data Sampling for Time Statistics is enabled in the Run Calculation

Task Page (p. ), ANSYS Fluent gathers data for time statistics while performing the simulation. The

statistics that ANSYS Fluent collects at each sampling interval (which consists of the mean and the

root-mean-square-error (RMSE) values) can be postprocessed by selecting Unsteady Statistics... in

any of the postprocessing dialog boxes. You can view several variables that include, but are not limited

to, shear stresses (Resolved UV/UW/VW Reynolds Stress), flow heat fluxes (Resolved UT/VT/WT Heat

Flux), and species statistics (RMSE Mass Fraction of species and Mean Mass Fraction of species). If

you select Unsteady Wall Statistics... in any of the postprocessing dialog boxes, you can view wall

statistics such as Mean Pressure Coefficient, Mean Wall Shear Stress, Mean X-Wall Shear Stress,

Mean Y-Wall Shear Stress, Mean Z-Wall Shear Stress, Mean Skin Friction Coefficient, Mean Surface

Heat Flux, Mean Surface Heat Transfer Coef., Mean Surface Nusselt Number, Mean Surface

Stanton Number. Note that these quantities are only the statistical evaluation of sampled solution

data, and do not contain any kind of modeled turbulent fluctuations. See Postprocessing for Time-

Dependent Problems (p. ) for details.

The Sampled Time field displays the time period over which data has been sampled for the postpro-

cessing of the mean and RMSE values. As long as the time step size has been constant, dividing this

by the time step size yields the number of data sets that have been collected. If the time step size is

varied, every contribution of data sets sampled is automatically weighted by the current time step

size.

Important

Note that mean statistics are collected only in interior cells and not on wall surfaces.

Therefore, when node or cell values of mean quantities are plotted on the wall surface, you

are actually plotting values in nearby cells attached to the wall.

If you want to control what set of variables are available for postprocessing, open the Sampling Options

dialog box and enable or disable the statistics shown in Figure . : The Sampling Options Dialog

Box (p. ).

Solution →

Run Calculation → Sampling Options...

Figure . : The Sampling Options Dialog Box

Important

When including or excluding statistics on variables, it is recommended that you re-initialize

the flow statistics.

You can use the postprocessing options not only for the purpose of interpreting your results but also

for investigating any anomalies that may appear in the solution. For instance, you may want to plot

contours of the  field to check if there are any regions where  is erroneously large or small. You

should see a high  region in the region where the production of  is large. You may want to display

the turbulent viscosity ratio field in order to see whether or not the turbulence takes full effect. Usually

the turbulent viscosity is at least two orders of magnitude larger than molecular viscosity for fully-de-

veloped turbulent flows modeled using the RANS approach (that is, not using LES). You may also want

to check whether you are using an adequate near-wall mesh when using a

insensitive wall treatment

(see Grid Resolution for RANS Models (p. ) for guidelines). For EWT- , you can also display filled

contours of

(turbulent Reynolds number) overlaid on the mesh (see Enhanced Wall Treatment ε-

Equation (EWT-ε) in the Theory Guide for more details).

Chapter : Modeling Heat Transfer

This chapter provides details about the heat transfer models available in ANSYS Fluent. Information is

presented in the following sections:

.. Modeling Conductive and Convective Heat Transfer

.. Modeling Radiation

.. Modeling Periodic Heat Transfer

The flow of thermal energy from matter occupying one region in space to matter occupying a different

region in space is known as heat transfer. Heat transfer can occur by three main mechanisms: conduction,

convection, and radiation. Physical models involving conduction and/or convection only are the simplest

(Modeling Conductive and Convective Heat Transfer (p. )), while buoyancy-driven flow or natural

convection (Natural Convection and Buoyancy-Driven Flows (p. )), and flow involving radiation

(Modeling Radiation (p. )) are more complex. Depending on your problem, ANSYS Fluent will solve

a variation of the energy equation that takes into account the heat transfer methods you have specified.

ANSYS Fluent is also able to predict heat transfer in periodically repeating geometries (Modeling Peri-

odic Heat Transfer (p. )), therefore greatly reducing the required computational effort in certain cases.

ANSYS Fluent allows you to include heat transfer within the fluid and/or solid regions in your model.

Problems ranging from thermal mixing within a fluid to conduction in composite solids can therefore

be handled by ANSYS Fluent.

When your ANSYS Fluent model includes heat transfer you will need to enable the relevant physical

models, supply thermal boundary conditions, and enter material properties (which may vary with tem-

perature) that govern heat transfer. For information about heat transfer theory, see Heat Transfer Theory

in the Theory Guide. Information about heat transfer theory and how to set up and use heat transfer

in your ANSYS Fluent model is presented in the following subsections:

... Solving Heat Transfer Problems

... Solution Strategies for Heat Transfer Modeling

... Postprocessing Heat Transfer Quantities

... Natural Convection and Buoyancy-Driven Flows

... Shell Conduction Considerations

The procedure for setting up a heat transfer problem is described below. Note that this procedure in-

cludes only those steps necessary for the heat transfer model itself; you will need to define the other

settings (for example, other models, boundary conditions) as usual.

. To activate the calculation of heat transfer, enable the energy equation by right-clicking Energy in the

tree (under Setup/Models) and clicking On in the menu that opens.

On

Figure . : Enabling the Energy Equation

. (Optional, pressure-based solver only.) If you are modeling viscous flow and you want to include the viscous

heating terms in the energy equation, enable the Viscous Heating option in the Viscous Model dialog

box.

Edit...

As noted in Inclusion of the Viscous Dissipation Terms in the Theory Guide, the viscous heating

terms in the energy equation are (by default) ignored by ANSYS Fluent when the pressure-based

solver is used. They are always included for the density-based solver. Viscous dissipation should

be enabled when the shear stress in the fluid is large (for example, in lubrication problems) and/or

in high-velocity, compressible flows. See Equation . in the Theory Guide.

. Define thermal boundary conditions at flow inlets, flow outlets, and walls.The boundary condition dialog

boxes can be opened by right-clicking the boundary name in the tree (under Setup/Boundary Conditions)

and clicking Edit... in the menu that opens; alternatively, you can open them from the Boundary Condi-

tions task page:

Setup →

At flow inlets and exits you will set the temperature; at walls you may use any of the following

thermal conditions:

specified heat flux

specified temperature

Modeling Heat Transfer

external radiation

combined external radiation and external convective heat transfer

Thermal Boundary Conditions at Walls (p. ) provides details on the model inputs that govern

these thermal boundary conditions. The default thermal boundary condition at inlets is a specified

temperature of  K; at walls the default condition is zero heat flux (adiabatic). See Cell Zone and

Boundary Conditions (p. ) for details about boundary condition inputs.

Important

If your heat transfer application involves two separated fluid regions, see the information

provided below.

. Define material properties for heat transfer.

Setup →

Materials

Heat capacity and thermal conductivity must be defined, and you can specify many properties as

Setup →

Materials

functions of temperature as described in Physical Properties (p. ).

.... Limiting the Predicted Temperature Range

For stability reasons, ANSYS Fluent includes a limit on the predicted temperature range. The purpose

of the temperature ceiling and floor is to improve the stability of calculations in which the temperature

should physically lie within known limits. Sometimes intermediate solutions of the equations give

rise to temperatures beyond these limits for which property definitions, and so on, are not well

defined.

The temperature limits keep the temperatures within the expected range for your problem. If the

ANSYS Fluent calculation predicts a temperature above the maximum limit, the stored temperature

values are “pegged” at this maximum value. The default for the temperature ceiling is  K. If the

ANSYS Fluent calculation predicts a temperature below the minimum limit, the stored temperature

values are “pegged” at this minimum value. The default for the temperature minimum is  K.

If you expect the temperature in your domain to exceed  K, use the Solution Limits dialog box

to increase the Maximum Static Temperature.

Limits...

.... Modeling Heat Transfer in Two Separated Fluid Regions

If your heat transfer application involves two fluid regions separated by a solid zone or a wall, as illus-

trated in Figure . : Typical Counterflow Heat Exchanger Involving Heat Transfer Between Two Sep-

arated Fluid Streams (p. ), you will need to define the problem with some care. Specifically:

You should not use outflow boundary conditions in either fluid.

You can establish separate fluid properties by selecting a different fluid material for each zone. For species

calculations, however, you can only select a single mixture material for the entire domain.

Modeling Conductive and Convective Heat Transfer

Figure . : Typical Counterflow Heat Exchanger Involving Heat Transfer Between Two Separated

Fluid Streams

Although many simple heat transfer problems can be successfully solved using the default solution

parameters assumed by ANSYS Fluent, you may accelerate the convergence of your problem and/or

improve the stability of the solution process using some of the guidelines provided in this section.

.... Under-Relaxation of the Energy Equation

When you use the pressure-based solver, ANSYS Fluent under-relaxes the energy equation using the

under-relaxation parameter defined by you in the Solution Controls task page, as described in Setting

Under-Relaxation Factors (p. ).

Solution →

Controls

If you are using the non-adiabatic non-premixed combustion model, you will set the energy under-

relaxation factor as usual but you will also set an under-relaxation factor for temperature, as described

below.

ANSYS Fluent uses a default under-relaxation factor of . for the energy equation, regardless of the

form in which it is solved (temperature or enthalpy). In problems where the energy field impacts the

fluid flow (via temperature-dependent properties or buoyancy) you should use a lower value for the

under-relaxation factor, in the range of .–.. In problems where the flow field is decoupled from

the temperature field (no temperature-dependent properties or buoyancy forces), you can usually

retain the default value of ..

.... Under-Relaxation of Temperature When the Enthalpy Equation is Solved

When the enthalpy form of the energy equation is solved (that is, when you are using the non-adia-

batic non-premixed combustion model), ANSYS Fluent also under-relaxes the temperature, updating

the temperature by only a fraction of the change that would result from the change in the (under-

relaxed) enthalpy values. This second level of under-relaxation can be used to good advantage when

you would like to let the enthalpy field change rapidly, but the temperature response (and its effect

on fluid properties) to lag. ANSYS Fluent uses a default setting of . for the under-relaxation on

temperature and you can modify this setting using the Solution Controls task page.

Solution →

Controls

.... Disabling the Species Diffusion Term

If you are solving for species transport using the pressure-based solver and you encounter convergence

difficulties, you may want to consider disabling the Diffusion Energy Source option in the Species

Model dialog box.

Setup → Models → Species

Edit...

When this option is disabled, ANSYS Fluent will neglect the effects of species diffusion on the energy

equation.

Note that species diffusion effects are always included when the density-based solver is used.

.... Step-by-Step Solutions

Often the most efficient strategy for predicting heat transfer is to compute an isothermal flow first

and then add the calculation of the energy equation. The procedure differs slightly, depending on

whether or not the flow and heat transfer are coupled.

..... Decoupled Flow and Heat Transfer Calculations

If your flow and heat transfer are decoupled (no temperature-dependent properties or buoyancy

forces), you can first solve the isothermal flow (energy equation turned off) to yield a converged

flow-field solution and then solve the energy transport equation alone.

Important

Since the density-based solver always solves the flow and energy equations together, the

procedure for solving for energy alone applies to the pressure-based solver, only.

You can temporarily disable the flow equations or the energy equation by deselecting them in the

Equations dialog box:

You can also disable the energy equation:

Off

..... Coupled Flow and Heat Transfer Calculations

If the flow and heat transfer are coupled (that is, your model includes temperature-dependent

properties or buoyancy forces), you can first solve the flow equations before enabling energy. Once

you have a converged flow-field solution, you can enable energy and solve the flow and energy

equations simultaneously to complete the heat transfer simulation.

.... Specifying a Solid Time step

For transient conjugate heat transfer (CHT) problems, particularly those with combustion, the dominant

time-scales in the fluid and solid zones are often quite different. In most cases, it is desirable to have

a larger time step in solid zones, while maintaining a smaller time step in fluid zones. This will increase

the speed at which the solid heat transfer reaches steady-state without compromising the solution

accuracy of the fluid flow.

You can specify a solid time step on the Run Calculation task page:

Figure . : The Run Calculation Task Page Showing Solid Time Step

. Under Options, select Solid Time Step.

. Use the default Automatic time step or select User Specified to enter your own time step.

..... Automatic Time Step Calculation

The default Automatic time step is calculated by ANSYS Fluent using the following formula:

(.)

where,

is the representative length scale and is calculated as

.

is

, the representative velocity scale, where  is the conductivity,  is the density, and

is the

specific heat capacity of the solid.

The calculation for

results in an approximation for the solid time step which might aide in

the solution running more efficiently. It should be noted, however, that this is only an engineering

approximation as there is no general way to calculate a meaningful length scale for an arbitrary

geometry.

For information about postprocessing heat transfer quantities, see the following sections:

.... Available Variables for Postprocessing

.... Definition of Enthalpy and Energy in Reports and Displays

.... Reporting Heat Transfer Through Boundaries

.... Reporting Heat Transfer Through a Surface

.... Reporting Averaged Heat Transfer Coefficients

.... Exporting Heat Flux Data

ANSYS Fluent provides reporting options for simulations involving heat transfer. You can generate

graphical plots or reports of the variables listed under the Temperature... or Wall Fluxes... category.

See Field Function Definitions (p. ) for the list of available variables and their definitions.

The reported enthalpy values may be different between the pressure-based and density-based solver

depending on the properties of the working fluid, compressible, incompressible, ideal gas, etc. For

details, see the discussion of enthalpy in The Energy Equation in chapter , Heat Transfer of the

You can use the Flux Reports dialog box to compute the heat transfer through each boundary of

the domain, or to sum the heat transfer through all boundaries to check the heat balance.

Results → Reports → Fluxes

Edit...

It is recommended that you perform a heat balance check to ensure that your solution is truly con-

verged.

Note

For the Composition PDF Transport model, the Flux Reports dialog box reports the Total

Heat Transfer Rate and Total Sensible Heat Transfer Rate only for the Lagrangian phase

solution, which does not always guarantee overall mass conservation due to the nature

of the discrete phase model. To check the balance of heat transfer rates that are based on

the continuous phase computation, you should use the Surface Integrals dialog box to

create a report for the Flow Rate of Enthalpy (Temperature category). (See Reporting

Heat Transfer Through a Surface (p. ) for details.)

You can use the Surface Integrals dialog box to compute the heat transfer through any boundary

or any surface created using the methods described in Creating Surfaces and Cell Registers for Dis-

playing and Reporting Data (p. ).

Results → Reports → Surface Integrals

Edit...

To report the mass flow rate of enthalpy

(.)

choose Flow Rate for the Report Type in the Surface Integrals dialog box, select Enthalpy (in the

Temperature... category) as the Field Variable, and select the surface(s) on which to integrate.

The Surface Integrals dialog box can also be used to generate a report of averaged heat transfer

coefficient  on a surface (

).

Edit...

In the Surface Integrals dialog box, choose Area-Weighted Average for Report Type, select Surface

Heat Transfer Coef. (in the Wall Fluxes... category) as the Field Variable, and select the surface.

It is possible to export heat flux data on wall zones (including radiation) to a generic file that you can

examine or use in an external program. To save a heat flux file, you will use the custom-heat-

flux text command.

file → export → custom-heat-flux

Heat transfer data will be exported in the following free format for each face zone that you select for

export:

zone-name nfaces

x_f y_f z_f A Q T_w T_c HTC

.

.

.

Each block of data starts with the name of the face zone (zone-name) and the number of faces in

the zone (nfaces). Next there is a line for each face (that is, nfaces lines), each containing the

components of the face centroid (x_f, y_f, and, in 3D, z_f), the face area (A), the heat transfer rate

(Q), the face temperature (T_w), the adjacent cell temperature (T_c), and the heat transfer coefficient

(HTC). If the heat transfer coefficient is calculated based on wall function (Equation . (p. )),

then

is the convective heat transfer rate. Otherwise,

will be the total heat transfer rate, including

radiation heat transfer.

When heat is added to a fluid and the fluid density varies with temperature, a flow can be induced

due to the force of gravity acting on the density variations. Such buoyancy-driven flows are termed

natural-convection (or mixed-convection) flows and can be modeled by ANSYS Fluent.

For more information about the theory behind natural convection and buoyancy-driven flows, see

Natural Convection and Buoyancy-Driven Flows Theory in the Theory Guide.

.... Modeling Natural Convection in a Closed Domain

When you model natural convection inside a closed domain, the solution will depend on the mass

inside the domain. Since this mass will not be known unless the density is known, you must model

the flow in one of the following ways:

Perform a transient calculation. In this approach, the initial density will be computed from the initial

pressure and temperature, so the initial mass is known. As the solution progresses over time, this mass

will be properly conserved. If the temperature differences in your domain are large, you must follow this

approach.

Perform a steady-state calculation using the Boussinesq model (described in The Boussinesq Model (p. )).

In this approach, you will specify a constant density, so the mass is properly specified.This approach is

valid only if the temperature differences in the domain are small. If not, you use the transient approach.

Important

For a closed domain, you can use the incompressible ideal gas law only with a fixed oper-

ating pressure. It cannot be used with a floating operating pressure. You can use the

compressible ideal gas law with either floating or fixed operating pressure.

See Floating Operating Pressure (p. ) for more information about the floating operating pressure

option.

....The Boussinesq Model

For many natural-convection flows, you can get faster convergence with the Boussinesq model than

you can get by setting up the problem with fluid density as a function of temperature. This model

treats density as a constant value in all solved equations, except for the buoyancy term in the mo-

mentum equation:

(.)

where

is the (constant) density of the flow,

is the operating temperature, and  is the thermal

expansion coefficient. Equation . (p. ) is obtained by using the Boussinesq approximation

(.)

where

to eliminate  from the buoyancy term. This approximation is accurate as long as

changes in actual density are small; specifically, the Boussinesq approximation is valid when

.

.... Limitations of the Boussinesq Model

The Boussinesq model should not be used if the temperature differences in the domain are large. In

addition, it cannot be used with species calculations, combustion, or reacting flows.

.... Steps in Solving Buoyancy-Driven Flow Problems

The procedure for including buoyancy forces in the simulation of mixed or natural convection flows

is described below.

tree (under Setup/Models) and clicking On in the menu that opens (Figure . : Enabling the Energy

Equation (p. )).

On

. Define the operating conditions in the Operating Conditions dialog box (Figure . :The Operating

Conditions Dialog Box (p. )).

Setup →

Figure . : The Operating Conditions Dialog Box

a.

Enable the Gravity option under Gravity.

b. Enter the appropriate values in the X, Y, and (for 3D) Z fields for Gravitational Acceleration for each

Cartesian coordinate direction. (Note that the default gravitational acceleration in ANSYS Fluent is

zero.)

c.

If you are using the incompressible ideal gas law, check that the Operating Pressure is set to an

appropriate (nonzero) value.

zero.)

c.

d. Depending on whether or not you use the Boussinesq approximation, specify the appropriate para-

meters described below:

If you are not using the Boussinesq model, the inputs are as follows:

i.

If necessary, enable the Specified Operating Density option in the Operating Conditions

dialog box, and enter a value for the Operating Density. See below for details.

ii.

Define the fluid density as a function of temperature as described in Defining Properties Using

Temperature-Dependent Functions (p. ) and Density (p. ).

Setup →

Materials

If you are using the Boussinesq model (described in The Boussinesq Model (p. )) the inputs are

i.

Enter the Operating Temperature (

in Equation . (p. )) in the Operating Conditions

ii.

Select boussinesq in the drop-down list for Density in the Create/Edit Materials dialog box

as described in Defining Properties Using Temperature-Dependent Functions (p. ) and

Density (p. ), and enter a constant value.

iii. Also in the Create/Edit Materials dialog box, enter an appropriate value for the Thermal Ex-

pansion Coefficient (  in Equation . (p. )) for the fluid material.

Note that if your model involves multiple fluid materials you can choose whether or not to

use the Boussinesq model for each material. As a result, you may have some materials using

the Boussinesq model and others not. In such cases, you will need to set all the parameters

described above in this step.

. Define the boundary conditions.The boundary condition dialog boxes can be opened by right-clicking

the boundary name in the tree (under Setup/Boundary Conditions) and clicking Edit... in the menu

that opens; alternatively, you can open them from the Boundary Conditions task page:

Setup →

The boundary pressures that you specify at pressure inlet and outlet boundaries are the redefined

pressures as given by Equation . (p. ). In general you should enter equal pressures,

, at

the inlet and exit boundaries of your ANSYS Fluent model if there are no externally imposed

pressure gradients.

. Set the parameters that control the solution, using the Solution Methods task page.

Solution →

Methods

a.

Select Body Force Weighted or Second Order in the drop-down list for Pressure under Spatial

Discretization in the Solution Methods task page.

b. If you are using the pressure-based solver, selecting PRESTO! for Pressure under Spatial Discretiz-

ation is recommended.

c.

Add cells near the walls to resolve boundary layers, if necessary.

See also Solving Heat Transfer Problems (p. ) for information on setting up heat transfer calculations.

.... Operating Density

When the Boussinesq approximation is not used, the operating density

appears in the body-force

term in the momentum equations as

. This form of the body-force term follows from the re-

definition of pressure in ANSYS Fluent as

(.)

The hydrostatic pressure in a fluid at rest is then

(.)

..... Setting the Operating Density

By default, ANSYS Fluent will compute the operating density by averaging over all cells. In some

(.)

cases, you may obtain better results if you explicitly specify the operating density instead of having

the solver compute it for you. For example, if you are solving a natural-convection problem with a

pressure boundary, it is important to understand that the pressure you are specifying is

in Equa-

tion . (p. ). Although you will know the actual pressure

, you will need to know the operating

density

in order to determine

from

. Therefore, you should explicitly specify the operating

density rather than use the computed average. The specified value should, however, be representative

of the average value.

In some cases the specification of an operating density will improve convergence behavior, rather

than the actual results. For such cases use the approximate bulk density value as the operating

density and be sure that the value you choose is appropriate for the characteristic temperature in

the domain.

Note that if you are using the Boussinesq approximation for all fluid materials, the operating density

does not appear in the body-force term of the momentum equation. Consequently, you need not

specify it.

.... Solution Strategies for Buoyancy-Driven Flows

For high-Rayleigh-number flows you may want to consider the solution guidelines below. In addition,

the guidelines presented in Solution Strategies for Heat Transfer Modeling (p. ) for solving other

heat transfer problems can also be applied to buoyancy-driven flows. No steady-state solution exists

for some laminar, high-Rayleigh-number flows.

..... Guidelines for Solving High-Rayleigh-Number Flows

When you are solving a high-Rayleigh-number flow (

), you should follow one of the procedures

outlined below for best results.

The first procedure uses a steady-state approach:

. Start the solution with a lower value of Rayleigh number (for example,

) and run it to convergence

using the first-order scheme.

. To change the effective Rayleigh number, change the value of gravitational acceleration (for example,

from . to . to reduce the Rayleigh number by two orders of magnitude).

. Use the resulting data file as an initial guess for the higher Rayleigh number and start the higher-Rayleigh-

number solution using the first-order scheme.

. After you obtain a solution with the first-order scheme you may continue the calculation with a higher-

order scheme.

The second procedure uses a time-dependent approach to obtain a steady-state solution  [] (p. ):

. Start the solution from a steady-state solution obtained for the same or a lower Rayleigh number.

. Estimate the time constant as  [] (p. )

(.)

where  and

are the length and velocity scales, respectively. Use a time step

such that

(.)

Using a larger time step

may lead to divergence.

. After oscillations with a typical frequency of

.–. have decayed, the solution reaches steady-

state. Note that  is the time constant estimated in Equation . (p. ) and  is the oscillation frequency

in Hz. In general this solution process may take as many as  time steps to reach steady-state.

.... Postprocessing Buoyancy-Driven Flows

The postprocessing reports of interest for buoyancy-driven flows are the same as for other heat

transfer calculations. See Postprocessing Heat Transfer Quantities (p. ) for details.

For information about shell conduction considerations, see the following sections:

.... Introduction

.... Physical Treatment

.... Limitations of Shell Conduction Walls

.... Managing Shell Conduction Walls

.... Initializing Shells

.... Locking the Temperature for Shells

.... Postprocessing Shells

By default, ANSYS Fluent treats walls as having zero-thickness and presenting no thermal resistance

to heat transfer across them. If a thickness is specified for a wall (thereby making it a thin wall, as

described in Thin-Wall Thermal Resistance Parameters (p. )) then the appropriate thermal resistance

across the wall thickness is imposed, although conduction is considered in the wall in the normal

direction only. There are applications, however, where conduction in the planar directions of the wall

is also important. For these applications, you have two options: you can either mesh the thickness,

or you can use the shell conduction approach. Shell conduction can be used to model one or more

layers of wall cells without the need to mesh the wall thickness in a preprocessor. When the shell

conduction approach is utilized, you have the ability to easily switch on and off conjugate heat

transfer on any wall. If you create a shell—either by enabling Shell Conduction in an individual Wall

dialog box (as described in Shell Conduction (p. )) or by defining multiple walls as shell conduction

zones using the Shell Conduction Manager dialog box (as described in Managing Shell Conduction

Walls (p. ))—and define the settings for the shell layer(s) using the Shell Conduction Layers dialog

box, then ANSYS Fluent will automatically grow the specified layers of cells. The cells that are grown

will be either prism cells or hex cells, depending on the type of face mesh that is utilized; at no point

are the cells visible in the displayed mesh.

Shell conduction can be used to account for thermal mass in transient thermal analysis problems (see

Locking the Temperature for Solid and Shell Zones (p. ) for more information). It can also be used

for multiple junctions and allows heat conduction through the junctions. Shell conduction can be

applied on boundary walls as well as two-sided walls.

In the case where shell conduction is applied on a boundary wall, the original surface is referred to

as the “wall surface” and is always adjacent to the fluid / solid cells. The first time the shell model is

enabled at any wall surface, Fluent grows the required shell zones. These layers are numbered sequen-

tially, starting with the one closest to the wall surface. See Figure . : A Boundary Wall with Shell

Conduction (p. ) for a visualization of how the solver treats shells.

For the most part, the boundary conditions that you specify for the boundary wall are applied to the

layer surface that is furthest from the wall surface; only the internal emissivity is applied at the wall

surface. The sides of the shell zone require boundary conditions as well. If the shell is connected to

another wall that does not have shell conduction enabled, the shell side will take the boundary con-

dition of the attached wall. The sides will be adiabatic if they are connected to face zones that have

a boundary condition type other than wall. If the attached wall has shell conduction enabled, then

the common sides at the junction will be coupled.

Figure . : A Boundary Wall with Shell Conduction

The layers of cells grown for two-sided walls can be visualized in a similar way to Figure . : A

Boundary Wall with Shell Conduction (p. ), except that the layer surface that is furthest from the

wall surface is also adjacent to a shadow wall (which is then adjacent to the other fluid / solid zone).

Figure . : A Two-Sided Wall with Shell Conduction

The following is a list of limitations for the shell conduction model:

Shells cannot be created on non-conformal interfaces, including mapped interfaces.

Shell conduction cannot be used on moving wall zones.

Shell conduction cannot be used with FMG initialization.

Shell conduction is not available when the wall is set up to receive thermal data via system coupling.

Shell conduction is not available for 2D.

Shell conduction is available only when the pressure-based solver is used.

Shell conducting walls cannot be split or merged. If you need to split or merge a shell conducting wall,

you will need to turn off the Shell Conduction option for the wall (in the Wall dialog box), perform the

split or merge operation, and then enable Shell Conduction for the new wall zones.

The shell conduction model cannot be used on a wall zone that has undergone hanging node adaption.

If you want to perform such adaption elsewhere in the computational domain, be sure to use a boolean

operation in an adaption expression to exclude a register containing the shell conducting walls. For example,

NOT(region_0). Refer to Adapting the Mesh (p. ) for additional information on adapting the mesh.

Fluxes at the ends of a shell conducting wall are not included in heat balance reports.These fluxes are

accounted for correctly in the ANSYS Fluent solution, but are not listed in the flux report.

The junction of a wall with shell conduction enabled and a non-conformal coupled wall is not supported.

When running the parallel solver with the shell conduction model, note that coupled walls are encapsulated.

If you encounter problems with the partitioning of the mesh, you can try changing the encapsulation

method to see if that resolves the problem (see Troubleshooting (p. ) for this and other troubleshooting

options).

Shells with a sharp bend may yield non-physical temperature fields when using Green-Gauss Node Based

gradients.This applies to any angle (acute or obtuse) with the effect worsening as the angle approaches

degrees.To resolve the issue, you should consider breaking the sharp angled shells into multiple shells

or, in the event that this cannot be done, enabling Warped Face Gradient Correction.

The Shell Conduction Manager dialog box provides a convenient way for you to manage, define,

and display multiple shell conduction zones. You can

display any wall zone

enable or disable shell conduction for a wall

define the settings for shell conduction walls or layers, such as thickness, material, and heat generation

rate

enable saving shell zones to case files.

Note that you can still enable shell conduction for a wall and define the related settings using the

Wall dialog box, as described in Shell Conduction (p. ). However, the Shell Conduction Manager

dialog box provides you with an alternative to do such activities from a single dialog box for all the

walls, instead of visiting the individual Wall boundary condition dialog boxes.

Physics → Model Specific → Shell Conduction...

Figure . : The Shell Conduction Manager Dialog Box

To manage shell conduction using the Shell Conduction Manager dialog box, perform the following

steps:

. (optional) If you have previously generated a CSV file that contains shell conduction settings for the

layers of the walls, you can read it by clicking Read... at the bottom of the Shell Conduction Manager

dialog box and using the dialog box that opens; otherwise, you should proceed to the steps that follow.

Using a CSV file can be helpful when you have a large number of layers and walls. It is not necessary

to create the CSV file from nothing, as you can create a simplified CSV file with sample values

using the Write... button (as described in step . ), and then revise the settings using a spreadsheet

program. See Shell Conduction Settings File Format (p. ) for details about the format of the

CSV file.

. Use the

and

buttons to move the selected zones from one list to another, and thereby define

whether they are shells. Zones with shell conduction enabled are listed under Shell Conduction Zones

and those without shell conduction are listed under Wall Zones. In essence, the

button disables

shell conduction and the

button enables shell conduction.

. Enable saving shell zones to case file is enabled by default so that Fluent automatically writes shell

zones into .cas files.When a case with shell zones is read back into Fluent, the shell zones will not need

to be recreated.

. Click the Display Zones button to display the selected walls in the graphics window. Note that you can

select walls with or without shell conduction.The zones will be displayed with different colors depending

on the option selected in the Mesh Colors dialog box, which is accessible from the Mesh Display dialog

box.

. Define settings for all of the shells by performing the following steps:

a.

Select walls from the Shell Conduction Zones for which you want to define the same settings.

b. Click the Settings... button to open the Shell Conduction Layers dialog box (Figure . : Shell

Conduction Layers Dialog Box (p. )).There you can specify the number of layers, and then define

the thickness, material, and heat generation rate for each layer. Note that you have the option of

defining the heat generation rate using a user-defined function (UDF) that utilizes the

DEFINE_PROFILE macro; for more information on creating and using user-defined functions, see

the Fluent Customization Manual.

Important

You must specify a nonzero-thickness for every layer.

Figure . : Shell Conduction Layers Dialog Box

c.

Click OK to save your settings for the selected walls and close the Shell Conduction Layers dialog

box.

. If you want to save all of the settings you specified using the Shell Conduction Manager dialog box as

a CSV file, click Write... and specify a name in the dialog box that opens.You can edit the shell conduction

settings in this CSV file using a spreadsheet program, and then read it in this or a separate case file, as

described in step . Note that information will not be written for any wall that defines the heat generation

rate using a UDF.

Note that you have the option of disabling shell conduction in every wall with a single action, by

using the following text command. This capability is available in both serial and parallel mode.

define → boundary-conditions → modify-zones → delete-all-shells

Shell zones can be patched using the Patch dialog box, as described in Patching Values in Selected

Cells (p. ).

Solution → Initialization

Patch...

You can lock (or “freeze”) the temperature values for all the cells in shells and solid zones (including

Patch...

those to which you have a hooked an energy source through a UDF) by using the solve/set/lock-

solid-temperature? text command, as described in Locking the Temperature for Solid and Shell

In order to facilitate the postprocessing of shells, surfaces (referred to as “shell surfaces”) are created

at the interface of adjacent layers, as well as at the layer surface that is furthest from the wall surface.

Note that shell surfaces are not created on the sides of the shell zones or in the interior of the layers.

The shell surfaces can then be selected from the Surfaces list available in a variety of dialog boxes

(for example, the Contours dialog box, the Surface Report Definition dialog box, and the Solution

XY Plot dialog box) in the same way as the surfaces for the wall and (for two-sided walls) the shadow

wall. When visualized in the graphics display window, these shell surfaces will be coincident with the

wall they are associated with.

The default naming convention for these shell surfaces is <wall_name>-<c0>:<c1>, where:

<wall_name> is the name of the wall on which the layers have been grown.

<c0> is the rank of the layer on the c0 side of the interface (that is, the layer closest to the wall surface).

<c1> is the rank of the layer on the c1 side of the interface (that is, the layer furthest from the wall surface).

Note that the layer surface that is furthest from the wall surface does not have a layer on the c1 side, and

so a different convention is used: for boundary walls, <c1> is set to external; for two-sided walls, <c1> is

set to the name of the fluid / solid adjacent to the shadow wall.

You have the ability to rename the shell surfaces, if you want. The following figures illustrate the default

naming convention, where the wall/shadow surfaces are displayed in red and the shell surfaces are

displayed in black.

Figure . : Shell Surface Names for a Boundary Wall

Figure . : Shell Surface Names for a Two-Sided Wall

You can use the walls, shadow walls, and shell surfaces to display the temperature of the interfaces

and adjacent cells. The Temperature... category provides two options: the temperature of the cell

on the c0 side of the surface is stored as Static Temperature; and the temperature of the surface itself

is stored as Wall Temperature. If a more detailed analysis of the solid zone and surfaces is required,

then you should consider creating layers of solid cells in your meshing application.

The following examples illustrate how to postprocess the surfaces shown in Figure . : Shell Surface

Names for a Boundary Wall (p. ):

The Static Temperature and Wall Temperature of Bwall will provide the temperature of the fluid cells

adjacent to Bwall and the temperature of the Bwall surface itself, respectively.

The Static Temperature and Wall Temperature of Bwall-: will provide the temperature of the cells

of Layer  and the temperature of the interface between Layer  and Layer  (that is, the Bwall-: shell

surface), respectively.

The Static Temperature and Wall Temperature of Bwall-:external will provide the temperature of the

cells of Layer  and the temperature of the layer surface that is furthest from the wall surface (that is, the

Bwall-:external shell surface), respectively.

Names for a Two-Sided Wall (p. ):

The Static Temperature and Wall Temperature of 2Swall-:air will provide the temperature of the cells

of Layer  and the temperature of the interface between Layer  and the shadow wall (that is, the 2Swall-

:air shell surface), respectively.

The Static Temperature and Wall Temperature of 2Swall-shadow will provide the temperature of the

air cells adjacent to 2Swall-shadow and the temperature of the shadow wall, respectively.

When postprocessing shells, note the following limitations:

You should not enable Node Values when postprocessing any surfaces associated with shells (that is, the

wall, shadow wall, or shell surfaces).The layers share nodes at the edges, and thus the averaging at such

nodes is erroneous.

You cannot postprocess shells in ANSYS CFD-Post, as shell surfaces are not supported.

Information about radiation modeling is presented in the following sections:

... Using the Radiation Models

... Setting Up the P- Model with Non-Gray Radiation

... Setting Up the DTRM

... Setting Up the S2S Model

... Setting Up the DO Model

... Setting Up the MC Model

... Defining Material Properties for Radiation

... Defining Boundary Conditions for Radiation

... Solution Strategies for Radiation Modeling

... Postprocessing Radiation Quantities

... Solar Load Model

For theoretical information about the radiation models in ANSYS Fluent, refer to Modeling Radiation in

The procedure for setting up and solving a radiation problem is outlined below, and described in detail

in referenced sections. Steps that are relevant only for a particular radiation model are noted as such.

The steps that are pertinent to radiation modeling, are shown here. For information about inputs related

to other models that you are using in conjunction with radiation, see the appropriate sections for

those models.

. Enable radiative heat transfer by selecting a radiation model (Rosseland, P1, Discrete Transfer (DTRM),

Surface to Surface (S2S), Discrete Ordinates, or Monte Carlo (MC)) under Model in the Radiation

Model dialog box (Figure . :The Radiation Model Dialog Box (DO Model) (p. )).

Setup → Models → Radiation

Edit...

Modeling Radiation

Figure . : The Radiation Model Dialog Box (DO Model)

Important

The Rosseland model can be used only with the pressure-based solver.

Note that when the P-, the DTRM, the S2S, DO, or MC model is enabled, the Radiation Model

dialog box expands to show additional parameters. These parameters will not appear if you select

the Rosseland model. If you are running a 3D case, you will have the added option of using the

solar load model. The solar load options will be displayed in the dialog box, below the radiation

model settings.

When the radiation model is active, the radiation fluxes will be included in the solution of the energy

equation at each iteration. If you set up a problem with the radiation model turned on, and you

then decide to turn it off completely, you must select the Off button in the Radiation Model dialog

box.

Note that when you enable a radiation model, ANSYS Fluent will automatically enable the energy

equation so that step is not needed.

. Set the appropriate radiation parameters.

a.

If you are modeling non-gray radiation using the P- model, define the non-gray radiation parameters

as described in Setting Up the P- Model with Non-Gray Radiation (p. ).

b. If you are using the DTRM, define the ray tracing as described in Setting Up the DTRM (p. ).

c.

If you are using the S2S model, define the surface clusters and view factors settings and compute or

read the view factors as described in Setting Up the S2S Model (p. ).

d. If you are using the DO model, choose DO/Energy Coupling if desired, define the angular discretization

as described in Setting Up the DO Model (p. ) and, if relevant, define the non-gray radiation para-

meters as described in Defining Non-Gray Radiation for the DO Model (p. ).

e. If you are using the MC model, specify the Target Number of Histories as described in Setting Up

the MC Model (p. ) and, if relevant, similar to when using the DO model, define the non-gray radiation

parameters as described in Defining Non-Gray Radiation for the DO Model (p. ).

. Define the material properties as described in Defining Material Properties for Radiation (p. ).

. Define the boundary conditions as described in Defining Boundary Conditions for Radiation (p. ). If

your model contains a semi-transparent medium, see the information below on setting up semi-transparent

media.

. Set the parameters that control the solution (DTRM, DO, MC, S2S, and P- only) as described in Solution

Strategies for Radiation Modeling (p. ).

. Run the solution as described in Running the Calculation (p. ).

. Postprocess the results as described in Postprocessing Radiation Quantities (p. ).

If you want to model non-gray radiation using the P- model, you can specify the Number of Bands

under Non-Gray Model in the expanded Radiation Model dialog box (Figure . : The Radiation

Model Dialog Box (Non-Gray P- Model) (p. )). By default, the Number of Bands is set to zero, indic-

ating that only gray radiation will be modeled. Because the cost of computation increases directly with

the number of bands, you should try to minimize the number of bands used. When a nonzero Number

of Bands is specified, the Radiation Model dialog box will expand once again to show the Wavelength

Intervals. For each wavelength band, you can specify a Name, as well as the Start and End wavelength

of the band in m. Note that the wavelength bands are specified for vacuum (

). For more inform-

ation about non-gray radiation calculations, see Defining Non-Gray Radiation for the DO Model (p. ).

Figure . : The Radiation Model Dialog Box (Non-Gray P- Model)

ANSYS Fluent allows you to use a user-defined function (UDF) to modify the emissivity weighting factor

(which otherwise defaults to the black body emission factor obtained from

a standard Planck distribution). The emissivity weighting factor appears in the emission term of the

radiative transfer equation for the non-gray model, as shown in Equation . in the Theory Guide.

For more information, see the Fluent Customization Manual.

For information about setting up the DTRM, see the following sections:

.... Defining the Rays

.... Controlling the Clusters

.... Controlling the Rays

....Writing and Reading the DTRM Ray File

.... Displaying the Clusters

When you select the Discrete Transfer model and click OK in the Radiation Model dialog box, the

DTRM Rays dialog box (Figure . : The DTRM Rays Dialog Box (p. )) will open automatically. If

you need to modify the current settings later in the problem setup or solution procedure, you can

open this dialog box by clicking DTRM Rays... in the Physics ribbon tab (Model Specific group box).

Figure . : The DTRM Rays Dialog Box

In this dialog box you will set parameters for and create the rays and clusters discussed in The DTRM

Equations in the Theory Guide.

. To control the number of radiating surfaces and absorbing cells, set the Cells Per Volume Cluster and

Faces Per Surface Cluster. (See the explanation below.)

. To control the number of rays being traced, set the number of Theta Divisions and Phi Divisions.

(Guidelines are provided below.)

. When you click OK in the DTRM Rays dialog box, The Select File Dialog Box (p. ) will open prompting

you for the name of the “ray file”. After you have specified the filename and chosen whether to write a

binary ray file, ANSYS Fluent will write the ray file and then read it afterward. During the write process

the status of the DTRM ray tracing will be reported in the ANSYS Fluent console. For example:

Completed % tracing of DTRM rays

Completed  % tracing of DTRM rays

See following sections for details on DTRM Rays dialog box inputs.

Important

If you cancel the DTRM Rays dialog box without writing and reading the ray file, the DTRM

will be disabled.

Your inputs for Cells Per Volume Cluster and Faces Per Surface Cluster will control the number of

radiating surfaces and absorbing cells. By default, each is set to , so the number of surface clusters

(radiating surfaces) will be the number of boundary faces, and the number of volume clusters (absorb-

ing cells) will be the number of cells in the domain. For small 2D problems, these are acceptable

numbers, but for larger problems you will want to reduce the number of surface and/or volume

clusters in order to reduce the ray-tracing expense. See Clustering in the Theory Guide for details

about clustering.

Note

Only zones attached to fluid cell zones are used for creating surface clusters.

Faces Per Surface Cluster (FPSC) is indicative of the actual reduction factor except when the

surfaces are planar.The surface clustering algorithm uses other criteria (angle between faces,

and so on) to ensure the clusters are nearly planar, so it is possible that there will be no further

reduction in the total number of clusters beyond a certain value of FPSC.

Your inputs for Theta Divisions and Phi Divisions will control the number of rays being traced from

each surface cluster (radiating surface).

Theta Divisions defines the number of discrete divisions in the angle  used to define the solid angle

about a point  on a surface. The solid angle is defined as  varies from  to  degrees (in the

Theory Guide), and the default setting of  for the number of discrete settings implies that there will

be one ray traced from the surface.

Phi Divisions defines the number of discrete divisions in the angle

used to define the solid angle

about a point  on a surface. The solid angle is defined as

varies from  to  degrees (Fig-

ure . : Angles θ and φ Defining the Hemispherical Solid Angle About a Point P in the Theory Guide).

The default setting of  implies that each ray traced from the surface will be located at a ° angle,

and in combination with the default setting for Theta Divisions, above, implies that  rays will be

traced from each surface control volume. In many cases, it is recommended that you at least double

the number of divisions in  and

.

After you have activated the DTRM and defined all of the parameters controlling the ray tracing, you

must create a ray file, which will be read back in and used during the radiation calculation. The ray

file contains a description of the ray traces (for example, path lengths, cells traversed by each ray).

This information is stored in the ray file, instead of being recomputed, in order to speed up the cal-

culation process.

By default, a binary ray file will be written. You can also create text (formatted) ray files by turning

off the Write Binary Files option in The Select File Dialog Box (p. ).

Important

Do not write or read a compressed ray file, because ANSYS Fluent will not be able to access

the ray tracing information properly from a compressed ray file.

The ray filename must be specified to ANSYS Fluent only once. Thereafter, the filename is stored in

your case file and the ray file will be automatically read into ANSYS Fluent whenever the case file is

read. ANSYS Fluent will remind you that it is reading the ray file after it finishes reading the rest of

the case file by reporting its progress in the console.

Note that the ray filename stored in your case file may not contain the full name of the directory in

which the ray file exists. The full directory name will be stored in the case file only if you initially read

the ray file through the GUI (or if you typed in the directory name along with the filename when using

the text interface). In the event that the full directory name is absent, the automatic reading of the

ray file may fail (since ANSYS Fluent does not know in which directory to look for the file), and you

will need to manually specify the ray file, using the File/Read/DTRM Rays... ribbon tab item. The

safest approaches are to use the GUI when you first read the ray file or to supply the full directory

name when using the text interface.

Important

You must recreate the ray file whenever you do anything that changes the mesh, such as:

change the type of a boundary zone

adapt the mesh

scale the mesh

You can open the DTRM Rays dialog box directly by clicking DTRM Rays... in the Physics

ribbon tab (Model Specific group box).

Once a ray file has been created or read in manually, you can click the Display Clusters button in

the DTRM Rays dialog box to graphically display the clusters in the domain. See Displaying Rays and

Clusters for the DTRM (p. ) for additional information about displaying rays and clusters.

When you select the Surface to Surface (S2S) model, the Radiation Model dialog box will expand

to show additional parameters (see Figure . : The Radiation Model Dialog Box (S2S Model) (p. )).

In these additional group boxes, you will set the solution parameters (see S2S Solution Parameters (p. )

for further details), access the view factors and clustering settings, and compute the view factors for

your problem or read previously computed view factors into ANSYS Fluent.

Figure . : The Radiation Model Dialog Box (S2S Model)

The S2S radiation model is very expensive in terms of computation effort and memory requirements

when there are a large number of radiating surfaces. You can reduce the number of radiating surfaces

by grouping faces together to form surface clusters. The surface cluster information (coordinates and

connectivity of the nodes, surface cluster IDs) is used by ANSYS Fluent in the radiosity calculations and

to compute the view factors.

Important

Important

You must recreate the surface cluster information whenever you do anything that changes the

mesh, such as:

– change the type of a boundary zone

– scale the mesh

Note that you do not need to recalculate view factors after shell conduction at any wall

has been enabled or disabled (see Thermal Boundary Conditions at Walls (p. ) for more

information about shell conduction). However, enabling or disabling shell conduction in

the parallel version of Fluent does cause a migration of cells and hence a change in the

partition. Whenever there is cell migration, the previously read view factor file is no longer

valid, and the view factor file must be read again using either the Read Existing File

button in the Radiation Model dialog box or the File/Read/View Factors... ribbon tab

item.

ANSYS Fluent will warn you to recreate the cluster/view factor file if a boundary zone has been

changed from a wall to an internal wall (or vice versa), or if a boundary zone has been merged,

separated, or fused.

....View Factors and Clustering Settings

You can use the View Factors and Clustering dialog box (Figure . : The View Factors and Clustering

Dialog Box (p. )) to define how the surface clusters are formed and how the view factors are calcu-

lated for the S2S model. To open this dialog box, click Settings... in the View Factors and Clustering

group box in the Radiation Model Dialog Box (p. ) (Figure . : The Radiation Model Dialog Box

(S2S Model) (p. )) or use the File/Write/Surface Clusters... ribbon tab item.

Figure . : The View Factors and Clustering Dialog Box

..... Forming Surface Clusters

You can set the number of faces per surface cluster (FPSC) for each flow boundary (that is, exhaust

fan, inlet vent, intake fan, outlet vent, mass-flow inlet, mass-flow outlet, pressure far-field, pressure

inlet, pressure outlet, outflow, and velocity inlet boundary) and wall that is adjacent to a fluid zone;

in this way, you can control the number of radiating surfaces and (if you select Cluster to Cluster

for Basis) view factor surfaces. By default, the FPSC value is set to  everywhere, so the number of

surface clusters (radiating/view factor surfaces) will be equal to the number of boundary faces. For

small 2D problems, this is an acceptable number. For larger problems, you may want to reduce the

number of surface clusters (that is, increase the FPSC) to reduce both the size of the view factor file

and the memory requirement. Such a reduction in the number of clusters, however, comes at the

cost of some accuracy. Note that for a thermally coupled mesh interface (that is, a fluid-fluid interface

with Coupled Wall enabled, or an interface involving a solid zone), the FPSC is always set to . See

Clustering in the Theory Guide for details about clustering.

Important

If you plan to use the cluster to cluster basis for the view factor calculation, be sure

that the FPSC values are appropriate for both the radiosity calculation and the view

factors.

Note that during the creation of a cluster on a non-conformal interface, its parent thread is taken

into the consideration; it may happen that the cluster is somewhat larger than its child face, which

may lead some inaccuracy in the flux calculation.

The Clustering group box in the View Factors and Clustering dialog box (Figure . : The View

Factors and Clustering Dialog Box (p. )) provides two methods for revising the default FPSC values:

manual

automatic

If you select Manual in the Options group box, you can specify an FPSC value for all flow boundaries

in the Faces per Surface Cluster for Flow Boundary Zones number-entry box in the Manual group

box. If you then click Apply to All Walls, you will apply this value to all wall zones that are adjacent

to fluid zones as well. For a wall that requires a different FPSC value (that is, you may want a lower

value for walls in critical areas, and higher values in non-critical areas), you will need to open the

boundary condition dialog box (Figure . : The Wall Dialog Box (p. )) for that particular wall

and modify the Faces Per Surface Cluster in the S2S Parameters group box of the Radiation tab.

Note that the Radiation tab also allows you to specify whether the wall participates in the view

factor calculation, as described in Specifying Boundary Zone Participation (p. ).

Note

Figure . : The Wall Dialog Box

Important

Important

The Faces Per Surface Cluster number-entry box will not be visible in the GUI on wall

boundary zones that are attached to a solid.

Using the manual method to specify the FPSC values for walls can become very cumbersome if the

model involves a large number of radiating faces, which is typically the case in underhood models.

In such circumstances, it is recommended that you use the automatic clustering method instead. In

this method, different FPSC values are assigned to the walls automatically, based on the distance of

the walls from and the FPSC values of the walls that are defined as critical. The steps you will need

to take are as follows:

. Select Automatic from the Options list in the View Factors and Clustering dialog box.

. For each wall that you deem critical, perform the following actions in the Wall dialog box (Fig-

ure . :The Wall Dialog Box (p. )):

a.

Click the Radiation tab.

b. Enter an appropriate value for Faces Per Surface Cluster in the S2S Parameters group box.

c.

Enable the Critical Zone option.

d. Click OK to close the Wall dialog box.

. Enter the Maximum Faces per Surface Cluster value in the View Factors and Clustering dialog box

and click the Compute button. ANSYS Fluent will automatically calculate and update the Faces Per

Surface Cluster values for all Wall dialog boxes adjacent to fluid zones that do not have Critical Zone

enabled, without computing the clusters.

. You can check the automatically assigned FPSC values by opening the boundary condition dialog box

of any non-critical wall of interest and examining the value for Faces Per Surface Cluster in the S2S

Parameters group box of Radiation tab.You can manually modify the value for Faces Per Surface

Cluster as necessary.

...... Setting the Split Angle for Clusters

Whether you set the FPSC value manually or automatically, you have the option of modifying the

cutoff or “split” angle between adjacent face normals for the purpose of controlling surface clustering.

The split angle sets the limit for which adjacent faces are clustered. A smaller split angle allows for

a better representation of the view factor. By default, no surface cluster will contain any face that

has a face normal greater than °. To modify the value of this parameter, you can use the split-

angle text command:

define → models → radiation → s2s-parameters → split-angle

or

file → write-surface-clusters → split-angle

..... Setting Up the View Factor Calculation

You can control many aspects of how the view factors are calculated for your S2S model: how surfaces

are defined; the computational method and related parameters; whether surface blocking will be

accounted for; and which boundary zones will participate in the calculation. All of these controls are

available in the View Factors group box in the View Factors and Clustering dialog box (Fig-

ure . : The View Factors and Clustering Dialog Box (p. )), and are described in the sections that

follow.

...... Selecting the Basis for Computing View Factors

ANSYS Fluent allows two ways to define the surfaces used for the view factor calculation, as described

in Clustering and View Factors in the Theory Guide. If you want the surfaces to be the boundary

faces of the mesh, select Face to Face for Basis in the View Factor group box of the View Factors

and Clustering dialog box. This is the default selection.

Alternatively, you can select Cluster to Cluster for Basis, in order to reduce the computational ex-

pense and storage requirements. In this case, the surfaces used to calculate the view factors are the

clusters defined by the settings in the Cluster group box of the View Factors and Clustering dialog

box. The reduction in computational time will be proportional to the number of surface clusters

used in the view factor calculation. The trade-offs of using the cluster to cluster basis for the calcu-

lation are that the accuracy may decrease, and the following limitations apply:

The mesh must be 3D.

You cannot subdivide the faces as part of the hemicube method parameters, which can cause the view

factors to be overestimated.

Polyhedral meshes are restricted to  face per surface cluster.

When using the cluster to cluster basis with non-conformal interfaces, the Faces Per Surface Cluster

will be limited to one, giving no advantage to the cluster to cluster basis.

...... Selecting the Method for Computing View Factors

ANSYS Fluent provides two methods for computing view factors: the ray tracing method (which is

selected by default) and the hemicube method. The following limitations apply:

The hemicube method is available only for 3D and axisymmetric cases.

The hemicube method should not be used when any of the zones are defined as periodic or symmetry

boundaries, as these types are not currently supported.

For the ray tracing method, when running in distributed parallel mode (including with Microsoft Job

Scheduler), the working directory must be shared across all machines.

The hemicube method uses a differential area-to-area method and calculates the view factors on a

row-by-row basis. The view factors calculated from the differential areas are summed to provide the

view factor for the whole surface. This method originated from the use of the radiosity approach in

the field of computer graphics  [] (p. ).

To use the hemicube method to compute the view factors, select Hemicube from the Method list

in the View Factors and Clustering dialog box. It is recommended that you use the hemicube

method for large, complex models with few obstructing surfaces between the radiating surfaces.

The hemicube method is based upon three assumptions about the geometry of the surfaces: aliasing,

visibility, and proximity. To validate these assumptions, you can specify three different hemicube

parameters, which can help you obtain better accuracy in calculating view factors. In most cases,

however, the default settings will be sufficient.

Aliasing—The true projection of each visible face onto the hemicube can be accurately accounted for

by using a finite-resolution hemicube. As described previously, the faces are projected onto a hemicube.

Because of the finite resolution of the hemicube, the projected areas and resulting view factors may be

overestimated or underestimated. Aliasing effects can be reduced by increasing the value of the Resol-

ution of the hemicube in the Parameters group box.

Visibility—The visibility between any two faces does not change. In some cases, face  has a complete

view of face  from its centroid, but some other face  occludes much of face  from face . In such a

case, the hemicube method will overestimate the view factor between face  and face  calculated from

the centroid of face .This error can be reduced by subdividing face  into smaller subfaces.You can

specify the number of subfaces by entering a value for Subdivisions in the Parameters group box. Note

that you cannot subdivide the faces when Cluster to Cluster is selected for Basis.

Proximity—The distance between faces is great compared to the effective diameter of the faces.The

proximity assumption is violated whenever faces are close together in comparison to their effective

diameter or are adjacent to one another. In such cases, the distances between the centroid of one face

and all points on the other face vary greatly. Since the view factor dependence on distance is nonlinear,

the result is a poor estimate of the view factor.

In the Parameters group box, you can set a limit for the Normalized Separation Distance, which

is the ratio of the minimum face separation to the effective diameter of the face. If the computed

normalized separation distance is less than the specified value, the face will then be divided into

a number of subfaces until the normalized distances of the subfaces are greater than the specified

value. Alternatively, you can specify the number of subfaces to create for such faces by entering

a value for Subdivisions.

While the hemicube method projects radiating surfaces onto a hemicube, the ray tracing method

instead traces rays through the centers of every hemicube face to determine which surfaces are

visible through that face. Note that the ray tracing method does not subdivide the faces (as can be

done when using the hemicube method by setting the Subdivisions or Normalized Separation

Distance parameters), and so the view factors may be less accurate than those calculated using the

hemicube method for surfaces that have a normalized separation distance less than .

To use the ray tracing method to compute the view factors, select Ray Tracing from the Method

list in the View Factors and Clustering dialog box. You can adjust the value of the Resolution in

the Parameters group box in order to reduce the impact of aliasing effects, as described previously.

...... Accounting for Blocking Surfaces

View factor calculations depend on the geometric orientations of surface pairs with respect to each

other. Two situations may be encountered when examining surface pairs:

If there is no obstruction between the surface pairs under consideration, then they are referred to as

“nonblocking” surfaces.

If there is another surface blocking the views between the surfaces under consideration, then they are

referred to as “blocking” surfaces. Blocking will change the view factors between the surface pairs and

require additional checks to compute the correct value of the view factors.

For cases with blocking surfaces, select Blocking from the Surfaces list in the View Factors and

Clustering dialog box. For cases with nonblocking surfaces, you can choose either Blocking or

Nonblocking without affecting the accuracy. However, it is better to choose Nonblocking for such

cases, as it takes less time to compute.

...... Specifying Boundary Zone Participation

You can choose to exclude walls and inlet and exit boundaries from participating in the view factor

calculation. If you are unsure whether it is necessary to calculate view factors for a particular

boundary zone ahead of time, it is recommended that you allow it to participate; you can always

reverse this decision as part of a future calculation run.

There are two ways in which you can enable/disable the participation of walls and inlet and exit

boundaries in the view factor calculation. One of those ways is to use the Participates in View

Factor Calculation option in the Radiation tab of the boundary condition dialog box. The other

method is to use the Participating Boundary Zones dialog box (Figure . : The Participating

Boundary Zones Dialog Box (p. )), which is accessed by clicking the Select... button next to the

Zones Participating in View Factor Calculation label in the View Factors and Clustering dialog

box. For cases that are made up of a very large number of zones, such as underhood applications,

the latter method is recommended.

Important

If you compute the view factors and then later alter which boundary zones participate in

the view factor calculation, you must recompute the view factors so that the data is up

to date.

Figure . : The Participating Boundary Zones Dialog Box

to date.

The Participating Boundary Zones dialog box allows you to easily specify those zones that are

participating or non-participating without having to visit the boundary conditions dialog box of

each zone. For cases that have a small number of boundary zones, you can simply select the zones

that you do not want to participate in the view factor calculation from the Participating Boundary

Zones list and click the arrow button that points to the right, so that the zones are moved to the

Non-Participating Boundary Zones list; if you make an error, you can always reverse this process

(that is, select a zone in the Non-Participating Boundary Zones list and click the arrow button that

points to the left). This can be cumbersome for cases that have a large number of boundary zones,

and so the following procedure is recommended instead:

. Make sure that your clustering options (see Forming Surface Clusters (p. )) are appropriate for your

view factor settings:

a.

Select Automatic from the Options list in the Clustering group box of the View Factors and

Clustering dialog box, as this enables some GUI items in the Participating Boundary Zones dialog

box.

Important

Note that if you do not want to use the Automatic option for the clustering, you

can revert to the Manual option after you are done using the Participating

Boundary Zones dialog box.

b. Verify that the walls you specified as critical (by enabling the Critical Zone option in the Radiation

tab of the boundary condition dialog box) also correspond to those that are critical for the view

factor calculation.You must have specified at least one critical zone for the steps that follow.

. Click the Compute button in the Maximum Distance from Critical Zone dialog box, to update the

value displayed for To All Other Zones.This value represents the maximum distance between the

centroids of a critical zone and a non-critical zone in the mesh; it is for information purposes only, and

cannot be edited in this dialog box.

. Based on the value displayed for To All Other Zones, enter a threshold value for To Participating

Zones.The value you enter will specify the maximum distance allowed between the centroids of a

critical zone and a zone that participates in the view factor calculation.Then click the Apply button to

move all zones beyond this distance into the Non-Participating Boundary Zones list.

. Review the zones displayed in the Participating Boundary Zones and Non-Participating Boundary

Zones lists. If necessary, select zones in these lists and use the arrow buttons to move them to the ap-

propriate list, as described previously.

If at any point you want to visually identify zones displayed in the Participating Boundary Zones

and Non-Participating Boundary Zones lists, select the zones and click the Display Zones button.

Only the selected zones will be displayed in the graphics window.

If any zones are displayed in the Non-Participating Boundary Zones list, ensure to enter an appro-

priate temperature for Non-Participating Boundary Zones Temperature. In most cases the appro-

priate value is the ambient temperature, which by default is assumed to be  K.

After you have specified which zones do not participate in view factor calculation and set their

temperature, click OK to store the settings and close the Participating Boundary Zones dialog box.

You can then proceed to computing the view factors, as described in the section that follows.

.... Computing View Factors

ANSYS Fluent can compute the view factors for your problem in the current session and save them

to a file for use in the current session and future sessions. Alternatively, you can save the surface

cluster information and view factor parameters to a file, calculate the view factors outside ANSYS

Fluent, and then read the view factors into ANSYS Fluent. These methods for computing view factors

are described in the following sections.

Important

For large meshes or complex models, it is recommended that you calculate the view factors

outside ANSYS Fluent and then read them into ANSYS Fluent before starting your simulation.

Note

You can accelerate view factor calculations by using ANSYS Fluent in parallel. For more

information see Accelerating View Factor Calculations for General Purpose Computing on

Graphics Processing Units (GPGPUs) (p. ).

..... Computing View Factors Inside ANSYS Fluent

To compute view factors in your current ANSYS Fluent session, you must first set the parameters for

the view factor calculation in the View Factors and Clustering dialog box (see View Factors and

Clustering Settings (p. ) for details) and click OK to save them. When you have set the view factor

and surface cluster parameters, click the Compute/Write/Read... button in the View Factors and

Clustering group box of the Radiation Model dialog box. A Select File dialog box will open,

prompting you for the name of the file in which ANSYS Fluent should save the surface cluster inform-

ation and the view factors. Note that the option to Write Binary Files is enabled by default, in order

to reduce the time needed to write and read the view factor files. When you click OK in the Select

File dialog box, ANSYS Fluent will write the surface cluster information to the file. ANSYS Fluent will

use the surface cluster information to compute the view factors, save the view factors to the same

file, and then automatically read the view factors. The ANSYS Fluent console will report the status

of the view factor calculation. For example:

Completed % calculation of view factors

Completed  % calculation of view factors

Important

You must recompute the view factors if you take any of following actions after the initial

computation:

– if you alter which boundary zones participate in the view factor calculation (either by using

the Participating Boundary Zones dialog box, or by enabling / disabling the Participates

in View Factor Calculation option in the Radiation tab of the boundary condition dialog

box)

– if you scale or unscale the mesh by using the Scale Mesh dialog box

The view factor file format for this version of ANSYS Fluent is known as the compressed row

box)

format (CRF) and is a more efficient way of writing view factors than in versions that are prior

to Fluent .. In the CRF format, only nonzero view factors with their associated cluster IDs

are stored to the file.This reduces the size of the .s2s file, and reduces the time it takes to

read the file into ANSYS Fluent.While the CRF file format is the default, you can still use the

older file format if necessary. Contact your support engineer for more information.

View factors using ray tracing are computed with the MPI/OpenMP hybrid model for parallel

runs. By default, one OpenMP thread is used per MPI process, as specified in the Thread

Control Dialog Box (p. ) (see Controlling the Threads (p. ) for details).To use all the

available cores on your machine as OpenMP threads, select Number of Cores on Machine.

A Fixed Number of cores can also be used based on your needs.

Note

For cases that use the S2S model and contain non-conformal interfaces, if the mesh

interfaces are defined after the case has been read, then the intersection of the inter-

face zones will occur during the initialization process, which will cause relabeling of

faces throughout the domain. If you attempt to compute view factors before solution

initialization in such a case, then the following message will be displayed in the

console and the view factors will be computed automatically during solution initial-

ization to avoid a mismatch with the case file:

Intersection zones for non-conformal interfaces are not created.

View factors will be computed during solution initialization.

..... Computing View Factors Outside ANSYS Fluent

To compute view factors outside ANSYS Fluent, you must save the surface cluster information and

view factor parameters to a file.

File → Write → Surface Clusters...

ANSYS Fluent will open the View Factors and Clustering dialog box, where you will set the view

factor and surface cluster parameters (see View Factors and Clustering Settings (p. ) for details).

When you click OK in the View Factors and Clustering dialog box, a Select File dialog box will

open, prompting you for the name of the file in which ANSYS Fluent should save the surface cluster

information and view factor parameters to the file. If the specified Filename ends in .gz or .Z,

appropriate file compression will be performed.

To calculate the view factors outside ANSYS Fluent, enter one of the following commands:

For the serial solver:

utility viewfac inputfile

where inputfile is the filename, or the correct path to the filename, for the surface cluster inform-

ation and view factor parameters file that you saved from ANSYS Fluent. You can then read the

view factors into ANSYS Fluent, as described below.

For the parallel solver:

– Viewfac utility module:

utility viewfac -t nprocs  [-p interconnect ] [-mpi= mpi_type ] [-cnf= hosts ] in-

putfile

where inputfile is the filename, for which you will need to provide the full path.

– Raytracing utility module:

utility raytracing -t nprocs  [-p interconnect ] [-mpi= mpi_type ] [-cnf= hosts

] [-ompthreads= N ] inputfile

On Windows:

tnprocs specifies the number of processes to use. When the -cnf option is present, the

hosts file argument is used to determine which machines to use for the parallel job. For ex-

ample, if there are  machines listed in the hosts file and you want to run a job with  processes,

set nprocs to  (that is -t4) and ANSYS Fluent will use the first  machines listed in the hosts

file. Note that this does not apply to the Compute Cluster Server (CCS).

pinterconnect (optional) specifies the type of interconnect. The ethernet interconnect is used

by default if the option is not explicitly specified. See Table . : Supported Interconnects for

the Windows Platform (p. ), Table . : Available MPIs for Windows Platforms (p. ), and

Table . : Supported MPIs for Windows Architectures (Per Interconnect) (p. ) for more in-

mpi=mpi_type (optional) specifies the type of MPI. If the option is not specified, the default

MPI for the given interconnect (IBM MPI) will be used (the use of the default MPI is recommen-

ded). The available MPIs for Windows are shown in Table . : Available MPIs for Windows

Platforms (p. ).

cnf=hosts (optional) specifies the hosts file, which contains a list of the machines on which

you want to run the parallel job. This option functions the same as that in the command for

launching parallel Fluent; see Starting Parallel ANSYS Fluent on a Windows System Using

Command Line Options (p. ) for details.

ompthreads=N (optional) specifies that the desired number of OpenMP threads to be used

per machine is N.

On Linux:

tnprocs specifies the number of processes to used. When the -cnf option is present, the

ample, if there are  machines listed in the hosts file and you want to run a job with  pro-

cesses, set nprocs to  (that is -t5) and ANSYS Fluent will use the first  machines listed in

the hosts file.

Linux Platforms (Per Platform) (p. ), Table . : Available MPIs for Linux Platforms (p. ),

and Table . : Supported MPIs for Linux Architectures (Per Interconnect) (p. ) for more in-

MPI for the given interconnect will be used (the use of the default MPI is recommended). The

available MPIs for Linux are shown in Table . : Available MPIs for Linux Platforms (p. ).

launching parallel Fluent; see Starting Parallel ANSYS Fluent on a Linux System Using Command

Line Options (p. ) for details.

.... Reading View Factors into ANSYS Fluent

If the view factors for your problem have already been computed (either inside or outside ANSYS

Fluent) and saved to a file, you can read them into ANSYS Fluent. To read in the view factors, click

Read Existing File... button in the View Factors and Clustering group box of the Radiation Model

dialog box. A Select File dialog box will open where you can specify the name of the file containing

the view factors. Alternatively, you can read the view factors file using the File/Read/View Factors...

Important

While the previous .s2s view factor file format can still be read seamlessly into ANSYS

Fluent, there is now a more efficient compressed row format (CRF) that can be read into

ANSYS Fluent (see the section on Computing View Factors Inside ANSYS Fluent). You can

take advantage of the reduced size of the CRF file and therefore the reduced time it takes

to read the file into ANSYS Fluent, by converting the existing old file format to the new

format (without having to recompute the view factors) using the following command at

the command prompt in your working directory:

utility viewfac -c1 -o new.s2s.gz old.s2s.gz

where new.s2s.gz is the CRF format to which you want the old file format (old.s2s.gz)

converted.

For information about setting up the DO model, see the following sections:

.... Angular Discretization

.... Defining Non-Gray Radiation for the DO Model

.... Enabling DO/Energy Coupling

For information about accelerating the DO solver, see Accelerating Discrete Ordinates (DO) Radiation

Calculations (p. ).

When you select the Discrete Ordinates model, the Radiation Model dialog box will expand to

show inputs for Angular Discretization (see Figure . : The Radiation Model Dialog Box (DO

Model) (p. )). In this section, you will set parameters for the angular discretization and pixelation

described in Angular Discretization and Pixelation in the Theory Guide.

Theta Divisions (

) and Phi Divisions (

) will define the number of control angles used to discretize

each octant of the angular space (see Figure . : Angular Coordinate System in the Theory Guide).

Note that higher levels of discretization are recommended for problems where specular exchange of

radiation is important to increase the likelihood of the correct beam direction being captured. For a

2D model, ANSYS Fluent will solve only  octants (due to symmetry); therefore, a total of

dir-

ections  will be solved. For a 3D model,  octants are solved, resulting in

directions . By

default, the number of Theta Divisions and the number of Phi Divisions are both set to . For most

practical problems, these settings are acceptable, however, a setting of  is considered to be a coarse

estimate. Increasing the discretization of Theta Divisions and Phi Divisions to a minimum of , or

up to , will achieve more reliable results. A finer angular discretization can be specified to better

resolve the influence of small geometric features or strong spatial variations in temperature, but larger

numbers of Theta Divisions and Phi Divisions will add to the cost of the computation.

Theta Pixels and Phi Pixels are used to control the pixelation that accounts for any control volume

overhang (see Figure . : Pixelation of Control Angle in the Theory Guide and the figures and discussion

preceding it). For problems involving gray-diffuse radiation, the default pixelation of

is usually

sufficient. For problems involving symmetry, periodic, specular, or semi-transparent boundaries, a

pixelation of

is recommended and will achieve acceptable results. The computational effort, as

a result of increasing the pixelation, is less than the computational effort caused by increasing the

divisions. You should be aware, however, that increasing the pixelation adds to the cost of computation.

Important

Note that pixelations are applied to boundary faces by default.

If you want to model non-gray radiation using the DO model, you can specify the Number of Bands

(

) under Non-Gray Model in the expanded Radiation Model dialog box (Figure . : The Radiation

Model Dialog Box (Non-Gray DO Model) (p. )). For a 2D model, ANSYS Fluent will solve

directions. For a 3D model,

directions will be solved. By default, the Number of Bands is

set to zero, indicating that only gray radiation will be modeled. Because the cost of computation in-

creases directly with the number of bands, you should try to minimize the number of bands used. In

many cases, the absorption coefficient or the wall emissivity is effectively constant for the wavelengths

of importance in the temperature range of the problem. For such cases, the gray DO model can be

used with little loss of accuracy. For other cases, non-gray behavior is important, but relatively few

bands are necessary. For typical glasses, for example, two or three bands will frequently suffice.

When a nonzero Number of Bands is specified, the Radiation Model dialog box will expand once

again to show the Wavelength Intervals (Figure . : The Radiation Model Dialog Box (Non-Gray

DO Model) (p. )). You can specify a Name for each wavelength band, as well as the Start and End

wavelength of the band in m. Note that the wavelength bands are specified for vacuum (

).

ANSYS Fluent will automatically account for the refractive index in setting band limits for media with

different from unity.

Figure . : The Radiation Model Dialog Box (Non-Gray DO Model)

The frequency of radiation remains constant as radiation travels across a semi-transparent interface.

The wavelength, however, changes such that

is constant. Therefore, when radiation passes from

a medium with refractive index

to one with refractive index

, the following relationship holds:

(.)

Here

and

are the wavelengths associated with the two media. It is conventional to specify the

wavelength rather than frequency. ANSYS Fluent requires you to specify wavelength bands (in m)

for an equivalent medium with

.

For example, consider a typical glass with a step jump in the absorption coefficient at a cut-off

wavelength of

. The absorption coefficient is

for

and

for

. The refractive index of

the glass is

. Since

for

and

for

. Since

is constant across a semi-transparent interface, the equivalent cut-off

wavelength for a medium with

is

using Equation . (p. ). You should choose two bands

in this case, with the limits  to

and

to . Here, the upper wavelength limit has been

chosen to be a large number, , in order to ensure that the entire spectrum is covered by the

bands. When multiple materials exist, you should convert all the cut-off wavelengths to equivalent

cut-off wavelengths for an

medium, and choose the band boundaries accordingly.

The bands can have different widths and need not be contiguous. You can ensure that the entire

spectrum is covered by your bands by choosing

and

. Here

and

are the minimum and maximum wavelength bounds of your wavelength bands, and

is the

minimum expected temperature in the domain.

ANSYS Fluent allows you to use a user-defined function (UDF) to modify the emissivity weighting

factor

(which otherwise defaults to the black body emission factor obtained

from a standard Planck distribution). The emissivity weighting factor appears in the emission term of

the radiative transfer equation for the non-gray model, as shown in Equation . in the Theory Guide.

For more information, see DEFINE_EMISSIVITY_WEIGHTING_FACTOR in the Fluent Customization

Manual.

For applications involving optical thicknesses greater than , you can enable the DO/Energy

Coupling option in the Radiation Model (Figure . : The Radiation Model Dialog Box with

DO/Energy Coupling Enabled (p. )) in order to couple the energy and intensity equations at each

cell, solving them simultaneously. This approach accelerates the convergence of the finite volume

scheme for radiative heat transfer and can be used with the gray or non-gray radiation model.

Figure . : The Radiation Model Dialog Box with DO/Energy Coupling Enabled

In the Iteration Parameters group box of the Radiation Model dialog box, you have the option of

revising the Target Number of Histories to be tracked for the Monte Carlo (MC) simulation. The default

value is ,. This can have a large effect on the accuracy of simulation results. For details, see

Monte Carlo Solution Accuracy in the Theory Guide.

In some cases, Fluent might calculate substantially more histories than the specified Target Number

of Histories, particularly if a fine surface mesh is used. The solver will ensure that an appropriate

minimum number of histories are started at each surface face, and that can increase the total number

of histories that are used during the calculation. Thus the CPU usage may not scale directly with

changes to the specified target.

In the Mesh Options group box, you can coarsen the radiation mesh by specifying a Target Cells Per

Volume Cluster greater than one. By default, it is set to one which implies no coarsening. Any value

greater than one reduces the number of effective cells in the domain used by the MC radiation model.

The coarsening is achieved by merging cells together and, therefore, does not affect the surface mesh

resolution or alter the faces of any merged cells. The reduction in cells may speed up the radiation

calculation and reduce peak memory usage, however, it may also have an impact on solution accuracy.

You have the option specifying multiple radiation bands using the Non-Gray Model group box. For

each desired band, you must specify a start and end wavelength similar to Defining Non-Gray Radiation

for the DO Model (p. ).

Figure . : The Radiation Model Dialog Box (MC)

When you are using the P-, DO, MC, or Rosseland radiation model in ANSYS Fluent, you should be

sure to define both the absorption and scattering coefficients of the fluid in the Create/Edit Materials

dialog box. Note that you can either enter a constant value for these parameters, or you can specify

them using a user-defined function (UDF). For more information, see DEFINE_PROPERTY UDFs in

Setup →

Materials

If you are modeling semi-transparent media using the DO or MC model, you should also define the

refractive index for the semi-transparent fluid or solid material. When using the Rosseland model, you

can specify the refractive index only for the fluid material. When using the P- model, you should

define the refractive index for the fluid material only. For the DTRM, you need to define only the ab-

sorption coefficient.

If your model includes gas phase species such as combustion products, absorption and/or scattering

in the gas may be significant. The scattering coefficient should be increased from the default of zero

if the fluid contains dispersed particles or droplets that contribute to scattering. Alternatively, you can

specify the scattering coefficient as a user-defined function (UDF). For more information, see

DEFINE_PROPERTY UDFs in the Fluent Customization Manual.

ANSYS Fluent allows you to enter a composition-dependent absorption coefficient for

and

mixtures, using the WSGGM. The method for computing a variable absorption coefficient is described

in Radiation in Combusting Flows in the Theory Guide. Radiation Properties (p. ) provides a detailed

description of the procedures used for specification of radiation properties.

.... Absorption Coefficient for a Non-Gray Model

If you are using the non-gray P-, DO, or MC model, you can specify a different constant absorption

coefficient for each of the bands used by the gray-band model, as described in Radiation Proper-

ties (p. ). You cannot, however, compute a composition-dependent absorption coefficient in each

band. If you use the WSGGM to compute a variable absorption coefficient, the value will be the same

for all bands. Alternatively, you can specify a user-defined function (UDF) for the absorption coefficient.

For more information, see DEFINE_PROPERTY UDFs in the Fluent Customization Manual.

.... Refractive Index for a Non-Gray Model

If you are using the non-gray P-, DO, or MC model, you can specify a different constant refractive

index for each of the bands used by the gray-band model, as described in Radiation Properties (p. ).

You cannot, however, compute a composition-dependent refractive index in each band.

When you set up a problem that includes radiation, you will set additional boundary conditions at inlets,

exits, and walls. These inputs are described in the sections that follow. The boundary condition dialog

boxes can be opened by right-clicking the boundary name in the tree (under Setup/Boundary Condi-

tions) and clicking Edit... in the menu that opens; alternatively, you can open them from the Boundary

Conditions task page:

Setup →

.... Inlet and Exit Boundary Conditions

..... Emissivity

When radiation is active, you can define the emissivity at each inlet and exit boundary when you

are defining boundary conditions in the associated inlet or exit boundary dialog box (for example,

Pressure Inlet dialog box, Velocity Inlet dialog box, Pressure Outlet dialog box). Enter the appro-

priate value for Internal Emissivity. The default value for all boundary types is . Alternatively, you

can specify a user-defined function for emissivity. For more information, see DEFINE_PROFILE in

For the non-gray P- model and the non-gray DO model, the specified constant emissivity will be

used for all wavelength bands.

Important

The Internal Emissivity boundary condition is not available with the Rosseland model.

..... Black Body Temperature

ANSYS Fluent includes an option that allows you to take into account the influence of the temperature

of the gas and the walls beyond the inlet/exit boundaries, and specify different temperatures for

radiation and convection at inlets and exits. This is useful when the temperature outside the inlet

or exit differs considerably from the temperature in the enclosure. For example, if the temperature

of the walls beyond the inlet is  K and the temperature at the inlet is  K, you can specify

the outside wall temperature to be used for computing radiative heat flux, while the actual temper-

ature at the inlet is used for calculating convective heat transfer. To do this, you would specify a

radiation temperature of  K as the black body temperature.

Although this option allows you to account for both cooler and hotter outside walls, you must use

caution in the case of cooler walls, since the radiation from the immediate vicinity of the hotter inlet

or outlet almost always dominates over the radiation from cooler outside walls. If, for example, the

temperature of the outside walls is  K and the inlet temperature is  K, it might be misleading

to use  K for the radiation boundary temperature. This temperature might be expected to be

somewhere between  K and  K; in most cases it will be close to  K. Its value depends

on the geometry of the outside walls and the optical thickness of the gas in the vicinity of the inlet.

In the flow inlet or exit dialog box (for example, Pressure Inlet dialog box, Velocity Inlet dialog

box), select Specified External Temperature in the External Black Body Temperature Method

drop-down list, and then enter the value of the radiation boundary temperature as the Black Body

Temperature.

Important

If you want to use the same temperature for radiation and convection, retain the default se-

Important

lection of Boundary Temperature as the External Black Body Temperature Method.

The Black Body Temperature boundary condition is not available with the Rosseland model.

....Wall Boundary Conditions for the DTRM, and the P-, S2S, and Rosseland

Models

The DTRM and the S2S, Rosseland, and gray P- (that is, Number of Bands is set to zero) models as-

sume all walls to be gray and diffuse. The only radiation boundary condition required in the Wall

dialog box is the emissivity. For the Rosseland model, the internal emissivity is . For the DTRM and

the S2S and gray P- models, you can enter the appropriate value for Internal Emissivity in the

Thermal tab of the Wall dialog box. The default value is . Alternatively, you can specify a user-defined

function for emissivity. For more information, see DEFINE_PROFILE in the Fluent Customization

Manual.

For the non-gray P– model, specify a constant Internal Emissivity for each wavelength band in the

Radiation tab of the Wall dialog box (the default value in each band is ). Alternatively, you can

specify the internal emissivity using a boundary condition parameter (see Creating a New Paramet-

er (p. )). See Defining Boundary Conditions for Radiation (p. ) for details.

..... Boundary Conditions for the S2S Model

When the S2S model is used, you can specify that some of the walls and inlet and exit boundaries

are not participating in the view factor calculation. This capability allows you to save time computing

the view factors and also reduce the memory required to store the view factor file during the ANSYS

Fluent calculation. See Specifying Boundary Zone Participation (p. ) for details.

Important

Whenever you revise which boundary zones participate in the calculation, you will need to

recompute the view factors.

The Flux Reports dialog box will not show the exact balance of the Radiation Heat Transfer

Rate because the radiative heat transfer to those boundaries that do not participate in the

view factor calculation is not included.

....Wall Boundary Conditions for the DO Model

When the DO model is used, you can model opaque walls, as discussed in Boundary and Cell Zone

Condition Treatment at Opaque Walls in the Theory Guide, as well as semi-transparent walls (Cell

Zone and Boundary Condition Treatment at Semi-Transparent Walls in the Theory Guide).

You can use a diffuse wall to model wall boundaries in many industrial applications since, for the

most part, surface roughness makes the reflection of incident radiation diffuse. For highly polished

surfaces, such as reflectors or mirrors, the specular boundary condition is appropriate. The semi-

transparent boundary condition can be appropriate, for example, when modeling for glass panes in

air.

..... Opaque Walls

In the Radiation tab of the Wall dialog box (Figure . : The Wall Dialog Box Showing Radiation

Conditions for an Opaque Wall (p. )), select opaque in the BC Type drop-down list to specify an

opaque wall.

Figure . : The Wall Dialog Box Showing Radiation Conditions for an Opaque Wall

Specify the fraction of reflected radiation flux that is to be treated as diffuse. By default, the Diffuse

Fraction is set to , indicating that all of the radiation is diffuse. A diffuse fraction equal to  indicates

purely specular reflected radiation. A diffuse fraction between  and  will result in partially diffuse

and partially specular reflected energy. If the non-gray DO model is being used, the Diffuse Fraction

can be specified for each band. See Boundary and Cell Zone Condition Treatment at Opaque Walls

in the Theory Guide for more details.

You will also be required to specify the internal emissivity in the Thermal tab of the Wall dialog

box (Figure . : The Wall Dialog Box Showing Internal Emissivity Thermal Conditions for an Opaque

Wall (p. )). For gray-radiation DO models, enter the appropriate value for Internal Emissivity

(default value is ). For non-gray DO models, specify a constant Internal Emissivity for each

wavelength band in the Radiation tab of the Wall dialog box. (The default value in each band is .)

Alternatively, you can specify the internal emissivity using a boundary condition parameter (see

Creating a New Parameter (p. )).

Figure . : The Wall Dialog Box Showing Internal Emissivity Thermal Conditions for an

Opaque Wall

You can also specify the external emissivity and external radiation temperature for an opaque wall

when the thermal conditions are set to Radiation or Mixed in the Wall dialog box (Figure . : The

Wall Dialog Box Showing External Emissivity and External Radiation Temperature Thermal Condi-

tions (p. )). Alternatively, you can specify a UDF for these parameters; for more information, see

DEFINE_PROFILE in the Fluent Customization Manual.

Figure . : The Wall Dialog Box Showing External Emissivity and External Radiation

Temperature Thermal Conditions

For more information on boundary condition treatment at opaque walls, see Boundary and Cell Zone

Condition Treatment at Opaque Walls in the Theory Guide.

..... Semi-Transparent Walls

To define radiation for an exterior semi-transparent wall, click the Radiation tab in the Wall dialog

box and then select semi-transparent in the BC Type drop-down list (Figure . : The Wall Dialog

Box for a Semi-Transparent Wall Boundary (p. )). The dialog box will expand to display the semi-

transparent wall inputs needed to define an external irradiation flux (Figure . : The Wall Dialog

Box for a Semi-Transparent Wall Boundary (p. )).

Figure . : The Wall Dialog Box for a Semi-Transparent Wall Boundary

. Specify the value of the irradiation flux (in W/m2) under Direct or Diffuse Irradiation. If the non-gray

DO model is being used, a constant Direct or Diffuse Irradiation can be specified for each band.

Important

Note that the external diffuse irradiation specified when using Radiation or Mixed

thermal conditions (selected in the Thermal tab), or Diffuse Irradiation (in the Radi-

ation tab) is always distributed hemispherically after transmission through semi-

transparent walls (that is independent of whether the external semi-transparent

boundary wall is defined as a diffusely or specularly reflecting type).

. Apply Direct Irradiation Parallel to the Beam is the default means of specifying the scale of irradiation

flux.When enabled, ANSYS Fluent assumes that the value of Direct Irradiation that you specify is the

irradiation flux parallel to the Beam Direction.When deselected, ANSYS Fluent instead assumes that

the value specified is the flux parallel to the face normals and will calculate the resulting beam parallel

flux for every face. See Figure . : DO Irradiation on External Semi-Transparent Wall in Semi-Transparent

Exterior Walls in the Theory Guide for details.

. Define the Beam Width by specifying the beam Theta and Phi extents. Beam width is specified as the

solid angle over which the irradiation is distributed.The default value for beam width is

, which is

suitable for collimated beam radiation. A beam width less than this is likely to result in zero irradiation

flux.

. Specify the (X,Y,Z) vector that defines the Beam Direction.The beam direction is defined as the vector

of the centroid of the solid angle (beam width).You can specify the Beam Direction as a constant, a

profile or a UDF.This is especially useful in applications where the shape of the radiative source is circular

or cylindrical (or nonlinear). For information about boundary profiles, see Reading and Writing Profile

Note that the actual direction of the beam of radiation that enters the domain will be further

influenced by the solid angles available from the number of divisions set up; the effective direction

will be the direction vector of the solid angle that the incoming beam falls into. Finally, any

nonzero diffuse fraction will act to spread out (hemispherically, proportional to the diffuse fraction)

the irradiation that enters the domain.

For a UDF example that specifies the beam direction, see Example  - Beam Direction Profile at

Semi-Transparent Walls in the Fluent Customization Manual.

. Specify the Diffuse Fraction, the fraction of the reflected radiation from the wall that is treated as diffuse

between  and  . By default, the Diffuse Fraction is set to , indicating that all of the radiation is diffuse.

A Diffuse Fraction of  treats the reflected radiation as purely specular. If you specify a value between

and  , the radiation is treated as partially diffuse and partially specular. If the non-gray DO model is

being used, the Diffuse Fraction can be specified for each band. See Diffuse Semi-Transparent Walls

Important

Note that the refractive index of the external medium is assumed to be .

If Heat Flux conditions are specified in the Thermal tab of the Wall dialog box, the specified

heat flux is considered to be only the conduction and convection portion of the boundary

flux.The given irradiation specifies the incoming exterior radiative flux; the radiative flux

transmitted from the domain interior to the outside is computed as a part of the calculation

by ANSYS Fluent. Internal emissivity is ignored for semi-transparent surfaces.

Note that when a boundary wall is made semi-transparent ANSYS Fluent calculates the amount

of radiation leaving as well as entering the domain. If you do not provide a source of irradiation

or a radiating thermal condition (for example Mixed or Radiation) then you are effectively

radiating to a temperature of  K and it is highly likely you may observe temperatures in your

model that are lower than expected. Ensure that the external (incoming) radiant conditions

give good account of the surroundings.

You can also specify the external emissivity and external radiation temperature for a semi-transparent

wall when the thermal conditions are set to Radiation or Mixed in the Wall dialog box (Fig-

ure . : The Wall Dialog Box Showing External Emissivity and External Radiation Temperature

Thermal Conditions (p. )). Alternatively, you can specify a user-defined function (UDF) for these

parameters; for more information, see DEFINE_PROFILE in the Fluent Customization Manual.

For a detailed description of boundary condition treatment at semi-transparent walls, see Cell Zone

and Boundary Condition Treatment at Semi-Transparent Walls in the Theory Guide.

To define radiation for an interior (two-sided) semi-transparent wall, in the Wall dialog box click the

Radiation tab and then select semi-transparent in the BC Type drop-down list (Figure . : The

Wall Dialog Box for an Interior Semi-Transparent Wall (p. )). Then specify the Diffuse Fraction as

described for the previous case.

Important

Important

Note that for semi-transparent walls, the internal emissivity defined under thermal condi-

tions is ignored. If you want to include the effect of internal emissivity at semi-transparent

walls, you must create a solid zone and specify that it participates in the radiation calcu-

lation; see Solid Semi-Transparent Media in the Theory Guide for details.

Figure . : The Wall Dialog Box for an Interior Semi-Transparent Wall

....Wall Boundary Conditions for the MC Model

When the MC model is used, you can model opaque walls and semi-transparent walls similar to the

DO model (see Wall Boundary Conditions for the DO Model (p. )) with some notable differences.

In the Radiation tab of the Wall dialog box (Figure . : The Wall Dialog Box for an Opaque Wall

with MC Model (Gray) (p. )), select opaque in the BC Type.

Figure . : The Wall Dialog Box for an Opaque Wall with MC Model (Gray)

For external walls, you have the option of specifying an external irradiation flux by selecting

Boundary Source. (Figure . : The Wall Dialog Box for an Opaque Wall with MC Model (Boundary

Source) (p. ))

. Specify the value of the irradiation flux (in W/m2) under Direct Irradiation. If the non-gray MC model

is being used, a constant Direct Irradiation can be specified for each band.

. Specify the (X,Y,Z) vector that defines the Beam Direction.To model an isotropic source, you must set

the Beam Direction to ,,.

Figure . : The Wall Dialog Box for an Opaque Wall with MC Model (Boundary Source)

Optionally select Polar Distribution Function, which can be used if the irradiation intensity varies

with direction, but is rotationally symmetric about a given direction. For example, LED light sources.

You have the option of specifying a polar distribution via an Expression or Table.

If you select Expression (Figure . : The Wall Dialog Box for an Opaque Wall with MC Model (Polar

Distribution with Expression) (p. )), enter an expression to define the polar distribution as a function

of "PolarAngle". For example:

cos(PolarAngle) + sin(PolarAngle)

The expression is evaluated at  angles between  and  degrees to form data pairs of Polar

Angle and Relative Intensity. You can write this polar distribution data via a .csv file or plot it to

the graphics window using the Write... and Plot... buttons, respectively.

If you select Table (Figure . : The Wall Dialog Box for an Opaque Wall with MC Model (Polar

Distribution with Table) (p. )), you must manually enter the data pairs or read a previously created

.csv file.

. Select the Number of Data Pairs to define the polar coordinate system for your irradiation source.

. Enter the data pairs in the form of Angle and Relative Intensity.

Note that the minimum number of data pairs is  and must include relative intensity data for

degrees. All angles must be between  and  degrees. Relative Intensity is typically between

and  although it does not have to be. A Relative Intensity of zero at a given angle means

there is no radiation in that direction.

. You have the option of reading and writing the polar distribution data (via .csv files) using the Read...

and Write... buttons.You can plot the polar distribution data in the graphics window by selecting

Plot....

Specify the (X,Y,Z) vector that defines the Reference Direction. This determines the center of the

polar distribution function.

Figure . : The Wall Dialog Box for an Opaque Wall with MC Model (Polar Distribution with

Expression)

Table)

Wall (Gray) (p. )). For gray-radiation MC models, enter the appropriate value for Internal

Emissivity.

Opaque Wall (Gray)

For the non-gray MC model, specify a constant Internal Emissivity for each wavelength band in

the Radiation tab of the Wall dialog box.

Figure . : The Wall Dialog Box for an Opaque Wall with MC Model (Non-gray)

You can also specify the external emissivity and external radiation temperature for an external wall

Specify the Diffuse Fraction, the fraction of the reflected radiation from the wall that is treated as

diffuse between  and  . By default, the Diffuse Fraction  is set to , indicating that all of the radi-

ation is diffuse. A diffuse fraction of  treats the radiation as purely specular. If you specify a value

between  and  , the radiation is treated as partially diffuse and partially specular. If the non-gray

MC model is being used, the Diffuse Fraction can be specified for each band.

For more information on boundary condition treatment at opaque walls (for the DO model), see

Boundary and Cell Zone Condition Treatment at Opaque Walls in the Theory Guide.

To define radiation for a semi-transparent wall, click the Radiation tab in the Wall dialog box and

then select semi-transparent in the BC Type.

For internal semi-transparent walls, specify the Internal Emissivity and Diffuse Fraction as described

in Opaque Walls (p. ).

For external semi-transparent walls, you also have the option of specifying external irradiation.

– If you enable Boundary Source and provide a beam direction, as described in Opaque Walls (p. ),

the external irradiation is treated as directional.

– If you specify the external emissivity and external radiation temperature for a semi-transparent wall

when the thermal conditions are set to Radiation or Mixed in the Wall dialog box (Figure . :The

Wall Dialog Box Showing Internal Emissivity Thermal Conditions for an Opaque Wall (Gray) (p. )),

the external irradiation is treated as diffuse.

Important

Important

Internal Emissivity is assumed to be zero for external semi-transparent walls. For Internal

semi-transparent walls, internal emissivity is only required on walls between fluid and solid

zones, or between two solid zones.

For a detailed description of boundary condition treatment at semi-transparent walls (for the DO

model), see Cell Zone and Boundary Condition Treatment at Semi-Transparent Walls in the Theory

Guide.

.... Solid Cell Zones Conditions for the DO or MC Models

With the DO or MC model, you can specify whether or not you want to solve for radiation in each

Guide.

cell zone in the domain. By default, the DO or MC equations are solved in all fluid zones, but not in

any solid zones. If you want to model semi-transparent media, for example, you can enable radiation

in the solid zone(s). To do so, enable the Participates In Radiation option in the Solid dialog box

(Figure . : The Solid Dialog Box (p. )).

Important

In general, you should not disable the Participates In Radiation option for any fluid zones.

See Solid Semi-Transparent Media in the Theory Guide for more information on solid semi-transparent

media.

....Thermal Boundary Conditions

In general, any well-posed combination of thermal boundary conditions can be used when any of

the radiation models is active. The radiation model will be well-posed in combination with fixed

temperature walls, conducting walls, and/or walls with set external heat transfer boundary conditions

(Thermal Boundary Conditions at Walls (p. )). You can also use any of the radiation models with

heat flux boundary conditions defined at walls, in which case the heat flux you define will be treated

as the sum of the convective and radiative heat fluxes. The exception to this is the case of semi-

transparent walls for the DO model. Here, ANSYS Fluent allows you to specify the convective and ra-

diative portions of the heat flux separately.

For the P-, DTRM, S2S, and the DO radiation models, there are several parameters that control the

radiation calculation. You can use the default solution parameters for most problems, or you can

modify these parameters to control the convergence and accuracy of the solution. Iteration parameters

that are unique for a particular radiation model are specified in the Radiation Model dialog box (for

example, Energy Iterations per Radiation Iteration). Spatial Discretization (Discretization in the

Theory Guide) and Under-Relaxation Factors (Under-Relaxation of Variables in the Theory Guide) are

specified in the Solution Methods and Solution Controls task pages, respectively. The Convergence

Criterion (Modifying Convergence Criteria (p. )) is set in the Residual Monitors dialog box.

There are no solution parameters to be set for the Rosseland model, since it impacts the solution only

through the energy equation.

Important

If radiation is the only model being solved in ANSYS Fluent and all other equations are

disabled, then the radiation transfer equation will automatically be solved for every iteration,

regardless of what the Energy Iterations per Radiation Iteration field is set to in the user

.... P- Model Solution Parameters

For the P- radiation model, you can control the convergence criterion and under-relaxation factor.

You should also pay attention to the optical thickness, as described below.

The default convergence criterion for the P- model is -, the same as that for the energy equation,

since the two are closely linked. See Monitoring Residuals (p. ) for details about convergence cri-

teria. You can set the Convergence Criterion for p1 in the Residual Monitors dialog box.

Solution → Monitors → Residuals

Edit...

The under-relaxation factor for the P- model is set with those for other variables, as described in

Setting Under-Relaxation Factors (p. ). Note that since the equation for the radiation temperature

(Equation . in the Theory Guide) is a relatively stable scalar transport equation, in most cases you

can safely use large values of under-relaxation (.–. ).

For optimal convergence with the P- model, the optical thickness

must be between .

and  (preferably not larger than ). Smaller optical thicknesses are typical for very small enclosures

(characteristic size of the order of  cm), but for such problems you can safely increase the absorption

coefficient to a value for which

. Increasing the absorption coefficient will not change

the physics of the problem because the difference in the level of transparency of a medium with

optical thickness = . and one with optical thickness <. is indistinguishable within the accuracy

level of the computation.

.... DTRM Solution Parameters

When the DTRM is active, ANSYS Fluent updates the radiation field during the calculation and computes

the resulting energy sources and heat fluxes via the ray-tracing technique described in Ray Tracing

in the Theory Guide. ANSYS Fluent provides several solution parameters in the expanded portion of

the Radiation Model dialog box (Figure . : The Radiation Model Dialog Box (DTRM) (p. )).

Figure . : The Radiation Model Dialog Box (DTRM)

You can control the maximum number of iterations of the radiation calculation during each global

iteration by changing the Maximum Number of Radiation Iterations. The default setting of  means

that the radiosity will be updated up to  times. The actual number of iterations will be less if the

residual convergence criterion is exceeded at any point during these iterations.

The Residual Convergence Criteria parameter (. by default) determines when the radiation in-

tensity update is converged. It is defined as the maximum normalized change in the surface intensity

from one DTRM radiation iteration to the next (see Equation . (p. )).

You can also control the frequency that the radiation field is updated as the continuous phase solution

proceeds. The Energy Iterations per Radiation Iteration parameter is set to  by default. This

means that the radiation calculation is performed once every  iterations of the solution process.

Increasing the number can speed the calculation process, but may slow overall convergence.

.... S2S Solution Parameters

For the S2S model, as for the DTRM, you can control the frequency with which the radiosity is updated

as the continuous-phase solution proceeds. See the previous description of Energy Iterations per

Radiation Iteration.

If you are using the pressure-based solver and you first solve the flow equations with the energy

equation turned off, you should reduce the Energy Iterations per Radiation Iteration from  to

or . This will ensure the convergence of the radiosity. If the default value of  is kept in this case,

it is possible that the flow and energy residuals may converge and the solution will terminate before

the radiosity is converged. See Residual Reporting for the S2S Model (p. ) for more information

about residuals for the S2S model.

The Residual Convergence Criteria (. by default) determines when the radiosity update is con-

verged. It is defined as the maximum normalized change in the radiosity from one S2S radiation iter-

ation to the next (see Equation . (p. )).

.... DO Solution Parameters

For the discrete ordinates model, as for the DTRM, you can control the frequency that the surface

intensity is updated as the continuous phase solution proceeds through the Energy Iterations per

Radiation Iteration setting. See the description of DTRM Solution Parameters (p. ).

For most problems, the default under-relaxation of . for the DO equations is adequate. For problems

with large optical thicknesses (

), you may experience slow convergence or solution oscillation.

For such cases, under-relaxing the energy and DO equations is useful. Under-relaxation factors between

. and . are recommended for both equations.

.... MC Solution Parameters

For the MC model, as for the DTRM, you can control the frequency that the surface intensity is updated

as the continuous phase solution proceeds through the Energy Iterations per Radiation Iteration

setting. See the description of DTRM Solution Parameters (p. ).

Wall Irradiation Flux.Normalized Std Deviation and Radiation Intensity.Nor-

malized Std Deviation (both available during postprocessing) can give an indication of the

quality of the solution. They arise from the stochastic nature of the Monte Carlo model.

Wall Irradiation Flux.Normalized Std Deviation is the maximum normalized standard

deviation of the irradiation flux at an element face on a boundary.The presence of small isolated boundary

regions with values of Wall Irradiation Flux.Normalized Std Deviation larger than %

is an indication that the element faces in those regions were insufficiently sampled. Increasing the Target

Number of Histories may help address this, at the expense of computational effort.

Radiation Intensity.Normalized Std Deviation is the maximum normalized standard

deviation of the radiation intensity within an element.The value of Radiation Intensity.Normal-

ized Std Deviation is expected to be less than % within a reliable radiation field solution.

Because of the stochastic behavior, it can be difficult to judge the convergence of MC radiation cases

based on residuals alone, particularly if the standard deviations are large. It is recommended that you

create a temperature probe (for example, a Surface Report Definition) and monitor its stability

during the solution. For more information, see Creating Report Definitions (p. ).

.... Running the Calculation

Once the radiation problem has been set up, you can proceed as usual with the calculation. Note

that while the P- and DO models will solve additional transport equations and report residuals, the

DTRM and the Rosseland and S2S models will not (since they impact the solution only through the

energy equation). Residuals for the DTRM and S2S model radiation iterations are reported by ANSYS

Fluent every time such an iteration is performed, as described below.

When running the S2S model with the parallel solver, note that coupled walls are encapsulated, which

may cause problems with the partitioning of the mesh. See Troubleshooting (p. ) for recommend-

ations on correcting such problems.

..... Residual Reporting for the P- Model

The residual for radiation as calculated by the P- model is updated after each iteration and reported

with the residuals for all other variables. ANSYS Fluent reports the normalized P- radiation residual

as defined in Monitoring Residuals (p. ) for the other transport equations.

..... Residual Reporting for the DO Model

After each DO iteration, the DO model reports a composite normalized residual for all the DO

transport equations. The definition of the residuals is similar to that for the other transport equations

(see Monitoring Residuals (p. )).

..... Residual Reporting for the DTRM

ANSYS Fluent does not include a DTRM residual in its usual residual report that is issued after each

iteration. The effect of radiation on the solution can be gathered, instead, via its impact on the energy

field and the energy residual. However, each time a DTRM iteration is performed, ANSYS Fluent will

print out the normalized radiation error for each DTRM radiation iteration. The normalized radiation

error is defined as

(.)

where the error  is the maximum change in the intensity ( ) at the current radiation iteration,

normalized by the maximum surface emissive power, and

is the total number of radiating surfaces.

Note that the default radiation convergence criterion, as noted in DTRM Solution Parameters (p. ),

defines the radiation calculation to be converged when  decreases to

or less.

..... Residual Reporting for the S2S Model

ANSYS Fluent does not include an S2S residual in its usual residual report that is issued after each

field and the energy residual. However, each time an S2S iteration is performed, ANSYS Fluent will

print out the normalized radiation error for each S2S radiation iteration. The normalized radiation

(.)

where the error  is the maximum change in the radiosity ( ) at the current radiation iteration,

is the total number of radiating surface

clusters. Note that the default radiation convergence criterion, as noted in DTRM Solution Paramet-

ers (p. ), defines the radiation calculation to be converged when  decreases to

or less.

..... Disabling the Update of the Radiation Fluxes

Sometimes, you may want to set up your ANSYS Fluent model with the radiation model active and

then disable the radiation calculation during the initial calculation phase. For the P- and DO models,

you can turn off the radiation calculation temporarily by deselecting P1 or Discrete Ordinates in

the Equations dialog box, which is accessed by right-clicking Solution Controls in the tree (under

Solution) and clicking Equations... in the menu that opens. For the DTRM and the S2S model, there

is no radiation calculation to disable in the Equations dialog box. You can instead set a very large

number for Energy Iterations per Radiation Iteration in the Iteration Parameters group box of

the Radiation Model dialog box.

If you turn off the radiation calculation, ANSYS Fluent will skip the update of the radiation field

during subsequent iterations, but will leave in place the influence of the current radiation field on

energy sources due to absorption, wall heat fluxes, and so on. Turning the radiation calculation off

in this way can therefore be used to initiate your modeling work with the radiation model inactive

and/or to focus the computational effort on the other equations if the radiation model is relatively

well converged.

Information regarding postprocessing radiation quantities can be found in the following sections:

.... Reporting Radiative Heat Transfer Through Boundaries

.... Overall Heat Balances When Using the DTRM

.... Displaying Rays and Clusters for the DTRM

.... Reporting Radiation in the S2S Model

ANSYS Fluent provides radiation quantities that you can use in postprocessing when your model in-

cludes the solution of radiative heat transfer. You can generate graphical plots or alphanumeric reports

of the following variables/functions:

In the Radiation... category:

Incident Radiation (P-, DO, and MC models)

Incident Radiation (Band n) (non-gray P-, non-gray DO, non-gray MC models)

Absorption Coefficient (DTRM, P-, DO, and Rosseland models)

Scattering Coefficient (P-, DO, and Rosseland models)

Refractive Index (P–, DO, and Rosseland models)

Radiation Temperature (P-, DO, and MC models)

Surface Cluster ID (S2S model)

Volumetric Absorbed Radiation (P-, DO, and MC models)

Volumetric Emitted Radiation (P-, DO, and MC models)

Radiation Intensity.Normalized Std Deviation (MC model)

Wall Irradiation Flux.Normalized Std Deviation (MC model)

In the Wall Fluxes... category:

Radiation Heat Flux (all radiation models)

Surface Incident Radiation (S2S, DTRM, and DO models)

Absorbed Radiation Flux (DO model, semi-transparent wall)

Reflected Radiation Flux (DO model, semi-transparent wall)

Transmitted Radiation Flux (DO model, semi-transparent wall)

Beam Irradiation Flux (DO model, semi-transparent wall)

See Field Function Definitions (p. ) for definitions of these postprocessing variables. Note that in

addition, incident radiation, transmitted, reflected and absorbed radiation flux are also available on

a per-band basis for the non-gray DO model.

Important

The sign convention on the radiative heat flux is such that the heat flux from the wall surface

is a positive quantity.

It is possible to export heat flux data on wall zones (including radiation) to a generic file that

you can examine or use in an external program. See Exporting Heat Flux Data (p. ) for details.

Take care not to confuse Incident Radiation and Surface Incident Radiation. Incident Radi-

ation is a volumetric quantity giving the total radiant load passing through the cell (in all dir-

ections), whereas Surface Incident Radiation is the total radiant load hitting the surface (which

will subsequently be absorbed, transmitted and reflected).There is no direct means to report

how much radiation has been absorbed/emitted/scattered in cells.

You can use the Flux Reports dialog box to compute the radiative heat transfer through each

boundary of the domain, or to sum the radiative heat transfer through all boundaries.

Edit...

See Fluxes Through Boundaries (p. ) for details about generating flux reports.

The DTRM yields a global heat balance and a balance of radiant heat fluxes only in the limit of a

sufficient number of rays. In any given calculation, therefore, if the number of rays is insufficient you

may find that the radiant fluxes do not obey a strict balance. Such imbalances are the inevitable

consequence of the discrete ray tracing procedure and can be minimized by selecting a larger number

of rays from each wall boundary.

When you use the DTRM, ANSYS Fluent allows you to display surface or volume clusters, as well as

the rays that emanate from a particular surface cluster. You can use the DTRM Graphics dialog box

(Figure . : The DTRM Graphics Dialog Box (p. )) for all of these displays.

Results → Model Specific → DTRM Graphics...

Figure . : The DTRM Graphics Dialog Box

..... Displaying Clusters

To view clusters, select Cluster under Display Type and then select either Surface or Volume under

Cluster Type.

To display all of the surface or volume clusters, select the Display All Clusters option under Cluster

Selection and click the Display button.

To display only the cluster (surface or volume) nearest to a specified point, deselect the Display All

Clusters option and specify the coordinates under Nearest Point. You may also use the mouse to

choose the nearest point. Click the Select Point With Mouse button and then right-click a point in

..... Displaying Rays

To display the rays emanating from the surface cluster nearest to the specified point, select Ray

under Display Type. Set the appropriate values for Theta and Phi Divisions under Ray Parameters

(see Setting Up the DTRM (p. ) for details), and then click the Display button. Figure . : Ray

Display (p. ) shows a ray plot for a simple 2D geometry.

Figure . : Ray Display

..... Including the Mesh in the Display

For some problems, especially complex 3D geometries, you may want to include portions of the

mesh in your ray or cluster display as spatial reference points. For example, you may want to show

the location of an inlet and an outlet along with displaying the rays. This is accomplished by enabling

the Draw Mesh option in the DTRM Graphics dialog box. The Mesh Display dialog box will appear

automatically when you enable the Draw Mesh option, and you can set the mesh display parameters

there. When you click Display in the DTRM Graphics dialog box, the mesh display, as defined in

the Mesh Display dialog box, will be included in the ray or cluster display.

When you use the S2S model, ANSYS Fluent allows you to view the values of the view factor and ra-

diation emitted from one zone to any other zone. You can use the S2S Information dialog box

(Figure . : The S2S Information Dialog Box (p. )) to generate a report of these values in the

console or as a separate file.

Results → Model Specific → S2S Information...

Figure . : The S2S Information Dialog Box

The steps for generating the report are as follows:

. Specify the values in which you are interested by selecting View Factors and/or Incident Radiation.

. Choose the zones for which you would like data by selecting them in the lists under From and To (at

least one zone must be selected under each list).To select all of the zones of a particular type, click that

category in the list under Boundary Types.

. Specify how you would like to present the data.To report the values in the console, click the Compute

button.To write the data as an S2S Info File (.sif format), click the Write... button and enter a file name

in The Select File Dialog Box (p. ).

The following is an example of how the data is presented:

S2S Information

From wall1 to:

View factor       Incident Radiation

wall1          . .

wall2          . .

wall3          . .

wall4          . .

From wall2 to:

wall1          . .

wall1          . .

wall2          . .

wall3          . .

wall4          . .

wall1          . .

wall2          . .

wall3          . .

wall4          . .

Note that the header listed above (S2S Information) is not displayed in the console.

ANSYS Fluent provides a solar load model that can be used to calculate radiation effects from the sun’s

rays that enter a computational domain. Two options are available for the model: Solar Ray Tracing

and Solar Irradiation. The Solar Ray Tracing approach is a highly efficient and practical means of ap-

plying solar loads as heat sources in the energy equations. In cases where you want to use the DO or

MC model to calculate radiation effects within the domain, the Solar Irradiation option is available to

supply outside beam direction and intensity parameters directly to the radiation model. The solar load

model includes a solar calculator utility that can be used to construct the sun’s location in the sky for

a given time-of-day, date, and position. Solar load is available in the 3D solver only, and can be used

to model steady and unsteady flows.

Typical applications that are well-suited for solar load simulations include the following:

automotive climate control (ACC) applications

human comfort modeling applications in buildings

The effects of solar loading are needed in many ACC applications, where the temperature, humidity,

and velocity fields around passengers (and drivers) are desired. ACC systems are tested for their capacity

to cool down passenger compartments after they have been “soaked” in intense solar radiation. ANSYS

Fluent’s solar load model will enable you to simulate solar loading effects and predict the time it will

take to reasonably cool down the cabin of a car that has been exposed to solar radiation, as well as

predict the time interval needed to lower the temperature in specified points and areas within the

domain.

In the analysis of buildings, solar loading provides a significant burden on the cooling requirement

in warm climates, particularly where architects want to use the aesthetics of glazed facades. Even in

cooler climates, solar loading can provide a burden during warmer seasons where modern buildings

are well insulated against thermal loss during winter months. As well as providing an engineer with

a practical tool for determining the solar heating effect inside a building, ANSYS Fluent’s solar load

model will allow the solar transmission through all glazed surfaces to be determined over the course

of a day, allowing important decisions to be made before undertaking any flow studies. ANSYS Fluent’s

solar load model also allows you to simulate porous blinds, which can transmit a portion of the solar

radiation while also allowing fluid flow.

.... Solar Ray Tracing

The solar load model’s ray tracing algorithm can be used to predict the direct illumination energy

source that results from incident solar radiation. It takes a beam that is modeled using the sun position

vector and illumination parameters, applies it to any or all wall, porous jump, and inlet/outlet

boundary zones that you specify, performs a face-by-face shading analysis to determine well-defined

shadows on all boundary faces and interior walls, and computes the heat flux on the boundary faces

that results from the incident radiation.

Important

The solar ray tracing model includes only boundary zones that are adjacent to fluid zones

in the ray tracing calculation. Therefore, boundary zones that are attached to solid zones

are treated as transparent and are not included in the ray tracing algorithm.

The resulting heat flux that is computed by the solar ray tracing algorithm is coupled to the ANSYS

Fluent calculation via a source term in the energy equation. The heat sources are added directly to

computational cells bordering each face and are assigned to adjacent cells in the following order:

shell conduction cells, solid cells, and fluid cells. Heat sources are assigned to one of these types of

adjacent cells, only. You can choose to override this order and include adjacent fluid cells in the solar

load calculation by issuing a command in the text user interface (see Text Interface-Only Com-

mands (p. ) for details). Note that the sun position vector and solar intensity can be entered either

directly by you or computed from the solar calculator. Direct and diffuse irradiation parameters can

also be specified using a user-defined function (UDF) and hooked to ANSYS Fluent in the Radiation

The solar ray tracing option allows you to include the effects of direct solar illumination as well as

diffuse solar radiation in your ANSYS Fluent model. A two-band spectral model is used for direct solar

illumination and accounts for separate material properties in the visible and infrared bands. A single-

band hemispherical-averaged spectral model is used for diffuse radiation. Opaque materials are

characterized in terms of two-band absorptivities. A semi-transparent material requires specification

of absorptivity and transmissivity. Values that you specify for transmissivity and absorptivity are

defined for normal incident rays. ANSYS Fluent recomputes/interpolates these values for the given

angle of incidence.

The solar ray tracing algorithm also accounts for internal scattered and diffusive loading. The reflected

component of direct solar irradiation is tracked. A fraction of this radiative heat flux, called internally

scattered energy is applied to all the surfaces participating in the solar load calculation, weighted by

area. The internally scattered energy depends on the scattering fraction that is specified in the TUI,

whose default value is . Depending on the reflectivity of the primary surface, the scattering fraction

can be responsible for the inclusion (or exclusion) of a large amount of radiation within the rest of

Also included as internally scattered energy is the contribution of the transmitted component of diffuse

solar irradiation (which enters a domain through semi-transparent walls depending upon the hemi-

spherical transmissivity). The total value of internally scattered energy is reported to the ANSYS Flu-

ent console. The ambient flux is obtained by dividing the internally scattered energy by the total

surface area of the faces participating in the solar load calculation.

Note that Solar Ray Tracing is not a participating radiation model. It does not deal with emission

from surfaces, and the reflecting component of the primary incident load is distributed uniformly

across all surfaces rather than being local to the surfaces reflected to. If surface emission is an important

factor in your case then you can consider implementing a radiation model (for example, P-) in con-

junction with Solar Ray Tracing.

Note the following limitation when using the solar ray tracing model:

Non-conformal interfaces are not supported with the solar ray tracing model.

..... Shading Algorithm

The shading calculation that is used for solar ray tracing is a straightforward application of vector

geometry. A ray is traced from the centroid of a test face in the direction of the sun. Every other

face is checked to determine if the ray intersects the candidate face and if the candidate face is in

front of the test face. If both conditions are met, then an opaque face completely shades the test

face. A semi-transparent face attenuates the incident energy.

A Barycentric coordinate formulation is used to construct triangle-ray intersections. A quadrilateral

ray intersection method is used to handle the case when model surfaces contain quadrilaterals. A

quad-tree preprocessing step is applied to reduce the ray tracing algorithm complexity that can lead

to long run times for

faces and greater. The quad-tree refinement factor can be modified in the

text interface. The default value of this parameter is , which is sufficient to cover the entire spectrum

of mesh sizes between one cell and five million cells. If the mesh is greater than five million cells,

an increase in this parameter would reduce the CPU time needed to compute the solar loads.

..... Glazing Materials

Incident solar radiation can be applied to glass and plastic glazing materials of various types at wall

boundaries, and the effects of coated glazings modeled using the solar ray tracing algorithm. To

model solar optical properties, you will need to specify the transmissivity and reflectivity of the

material in the Wall boundary conditions dialog box. You can obtain these values from the glass (or

plastic) manufacturer or use data from another source (for example, ASHRAE Handbook).

Glazing optical properties are dependent on incident angle, and the variation is significant for an

incident angle greater than

degrees. As the incident angle increases from zero, transmissivity

decreases, reflectivity increases, and absorptivity increases initially due to lengthened optical path,

and then decreases as more incident radiation is reflected. The shape of the property curve varies

with glass type and thickness. This difference is more pronounced for coated glass or for a multiple-

pane glazing system. It cannot be assumed that all glazing systems have a universal angular depend-

ence.

For coated glazings, the spectral transmissivity and reflectivity at any incident angle are approximated

in the solar load model from the normal angle of incidence  [] (p. ).

Transmissivity is given by

(.)

where

(.)

Reflectivity is given by

(.)

where

(.)

(.)

where

(.)

(.)

where

(.)

The constants used in Equation . (p. ) and Equation . (p. ) are for coated glazings and

are taken from Finlayson and Arasteh. [] (p. ). The normal transmissivity and reflectivity,

and

are specified in the Wall boundary conditions dialog box.

..... Inputs

The following inputs are required for the solar ray tracing algorithm:

sun direction vector

direct solar irradiation

diffuse solar irradiation

spectral fraction

direct and IR absorptivity (opaque wall)

direct and IR absorptivity and transmissivity (semi-transparent wall and porous jump)

diffuse hemispherical absorptivity and transmissivity (semi-transparent wall)

solar transmissivity factor

quad tree refinement factor

scattering fraction

ground reflectivity

The sun direction vector is the direction vector looking to the sun, from which the direct irradiation

will be incident. You can enter the vector components (X, Y, Z) and the direct and diffuse solar irra-

diation fluxes in the Radiation Model dialog box, or you can have these parameters derived from

the solar calculator. These irradiation fluxes can also be specified using a user-defined function (User-

Defined Functions (UDFs) for Solar Load (p. )). The spectral fraction is the final input in the Radi-

ation Model dialog box. This defines the split of visible and infra-red (shortwave and longwave re-

spectively) radiation, specifically the fraction of the direct irradiation flux that is in the visible band.

These quantities can also be defined through the text interface.

The scattering fraction defines the amount of non-absorbed radiation that will be distributed (uni-

formly) across all participating surfaces. This is required as the solar load model does not track the

rays beyond the first opaque surface. Therefore, a highly glazed space where incident radiation is

likely to be reflected back out will have a low value. Conversely, a predominantly opaque (wall-

bounded) space where reflected radiation is likely to be incident upon (and ultimately absorbed by)

other opaque surfaces will have a high value. This parameter is defined through the text interface

only, taking a default value of . :

define → models → radiation → solar-parameters → scattering-fraction

The ground reflectivity is used by the solar calculator to compute the background diffuse radiation

intensity component contributed to by radiation reflected off the ground. This should be based on

typical figures for the surface reflectivity of the outside ground surfaces. By default this is set to .,

but can be adjusted through the text-interface:

define → models → radiation → solar-parameters → ground-reflectivity

The quad-tree-refinement parameter determines the level of detail used by the shading algorithm.

By default this is set to  which will generally work well, but can lie between  and . This is defined

only through the text interface:

define → models → radiation → solar-parameters → quad-tree-refinement

Further details on the text interface-only entries is provided later in this section (see Text Interface-

Only Commands).

The absorptivity and transmissivity parameters related to a wall or porous jump are entered in the

Wall (under the Radiation tab) or Porous Jump boundary condition dialog box, respectively, for

the particular boundary zones you want to participate in solar ray tracing. On flow boundaries you

have a solar transmissivity factor to allow you to attenuate the incoming solar flux, for example, set

to  for a fully open inlet or set to  for a light obscuring louvered inlet.

.... Solar Irradiation

The solar load model’s Solar Irradiation option provides you with an easy means of applying a solar

load directly to the DO or MC model. Unlike the ray tracing solar load option, the Solar Irradiation

method does not compute heat fluxes and apply them as heat sources to the energy equation. Instead,

the irradiation flux is applied directly to semi-transparent walls (which you specify) as a boundary

condition, and the radiative heat transfer is derived from the solution of the radiation model itself.

The following inputs are required for Solar Irradiation at semi-transparent walls:

direct irradiation

diffuse irradiation (not available for MC model)

beam direction

beam width (only required for DO model)

diffuse fraction

In the Wall boundary condition dialog box for each semi-transparent wall you want to participate in

Solar Irradiation, you can specify that the beam direction, direct irradiation, and diffuse irradiation be

derived from the solar parameters (for example, solar calculator) that you set (or compute) in the

Radiation Model dialog box. This is done by checking the Use Beam Direction from Solar Load

Model Settings and Use Irradiation from Solar Load Model Settings boxes. When selected, ANSYS

Fluent sets the beam width (the angle subtended by the sun) to the default value of

degrees

when using the DO model.

Important

Note that the sign of the beam direction that is needed for the DO or MC model is opposite

the sun direction vector that is entered or derived from the solar parameters. The beam

direction in the DO or MC model is the direction of external radiation (for example, radiation

coming from the sun), while the sun direction vector in the solar load model points to the

sun.

.... Solar Calculator

ANSYS Fluent provides a solar calculator that can be used to compute solar beam direction and irra-

diation for a given time, date, and position. These values can be used as inputs to the solar ray tracing

algorithm or as semi-transparent wall boundary conditions for solar irradiation.

..... Inputs/Outputs

Inputs needed for the solar calculator are:

global position (latitude, longitude, time zone)

starting date and time

mesh orientation

solar irradiation method

sunshine factor

Global position consists of latitude, longitude, and time zone (relative to GMT). The time of day for

a transient simulation is the starting time plus the flow-time. For mesh orientation, you will need to

specify the North and East direction vector in the CFD mesh. The default solar irradiation method is

Fair Weather Conditions. Alternatively, you can choose the Theoretical Maximum method. The sunshine

factor is simply a linear reduction factor for the computed incident load that allows for cloud cover

to be accounted for, if appropriate.

You can specify these inputs in the Solar Calculator dialog box that is accessible from the Radiation

Model dialog box (Figure . : The Solar Calculator Dialog Box (p. )). Alternatively, you can enter

the parameters using text interface commands (Additional Text Interface Commands (p. )).

The following values are computed by the solar calculator and are displayed in the console

whenever the solar calculator is used:

sunshine fraction

direct normal solar irradiation at earth’s surface

diffuse solar irradiation - vertical and horizontal surface

ground reflected (diffuse) solar irradiation - vertical surface

Direct normal solar irradiation is computed using the ASHRAE Fair Weather Conditions method,

when this option is selected in the solar calculator. Note: Equation  and Table  from Chapter

of the  ASHRAE Handbook of Fundamentals. The theoretical maximum values for direct normal

solar irradiation and diffuse solar irradiation are computed using NREL’s Theoretical Maximum

method, when this option is selected. In practice, these values are unlikely to be experienced due

to atmospheric conditions.

ANSYS Fluent computes the diffuse solar irradiation components (vertical and horizontal) internally

for each face in the domain. When the Theoretical Maximum method is chosen, these diffuse irradi-

ation values provide estimates for the maximum vertical and horizontal surface effects.

.....Theory

ANSYS Fluent provides two options for computing the solar load: Fair Weather Conditions method

and Theoretical Maximum method. Although these methods are similar, there is a key difference.

The Fair Weather Conditions method imposes greater attenuation on the solar load, which is repres-

entative of atmospheric conditions that are fair–but not completely clear.

The equation for normal direct irradiation applying the Fair Weather Conditions Method is taken

from the ASHRAE Handbook:

(.)

where  and  are apparent solar irradiation at air mass

and atmospheric extinction coefficient,

respectively. These values are based on the earth’s surface on a clear day.

is the solar altitude (in

degrees) above the horizontal.

The equation for direct normal irradiation that is used for the Theoretical Maximum Method is taken

from NREL’s Solar Position and Intensity Code (Solpos):

(.)

where

is the top of the atmosphere direct normal solar irradiance and

is the correction

factor used to account for reduction in solar load through the atmosphere.

The calculation for the diffuse load in the solar model is based on the approach suggested in the

ASHRAE Fundamental Handbook (Chapter , Fenestration). The equation for diffuse solar irra-

diation on a vertical surface is given by:

(.)

where  is a constant whose values are given in Table  from Chapter  of the  ASHRAE

Handbook of Fundamentals,

is the ratio of sky diffuse radiation on a vertical surface to that on a

horizontal surface (calculated as a function of incident angle), and

is the direct normal irradiation

at the earth’s surface on a clear day.

The equation for diffuse solar irradiation for surfaces other than vertical surfaces is given by:

(.)

where  is the tilt angle of the surface (in degrees) from the horizontal plane.

The equation for ground reflected solar irradiation on a surface is given by:

(.)

where

is the ground reflectivity. The total diffuse irradiation on a given surface will be the sum

of

and

when the input for diffuse solar radiation is taken from the solar calculator. Otherwise,

if the constant option is selected in the Radiation dialog box, then the total diffuse irradiation

will be the same as specified in the dialog box.

..... Computation of Load Distribution

In calculating the solar load that will be incident on each surface, it is necessary to distinguish

between the calculation of diffuse and direct solar loads. A direct load will be tracked from particip-

ating transmissive boundary surfaces and non-participating boundary surfaces, the former provides

some opportunity to attenuate the incoming flux by absorption and reflection, while the non-parti-

cipating surfaces allow the flux to enter without any drop in intensity. The direct load is then tracked

through the model space until it is incident on an opaque surface, or it exists through a transmissive

or non-participating boundary zone. During its passage, its intensity will be attenuated as it passes

through participating semi-transparent internal walls, where some radiation may be absorbed and

some may be reflected. The total amount of direct radiation that is reflected at internally facing

surfaces will be added to the scattered radiation budget for further use later.

The diffuse load originates at participating transmissive boundary surfaces. It is these surfaces that

permit diffuse radiation to enter, irrespective of their orientation relative to the direction vector. For

each transmissive surface, some of the incoming diffuse load may be immediately absorbed and/or

reflected to the outside. The rest is assumed to be transmitted inside and summed from all of these

surfaces to give an initial diffuse budget. Onto this budget is added a fraction of the previously

computed scattered radiation from the direct load, the fraction used is defined as an input to the

model. This provides the total diffuse load. This is then uniformly distributed across all surfaces that

are participating in the solar calculation, irrespective of whether they are opaque or semi-transparent.

There is no scope to define local absorptivity for this distribution and no biasing with regards prox-

imity to transmissive surfaces. Note that a non-participating boundary zone will allow direct load to

enter the model space but will not provide an incoming quantity of diffuse load.

Note that the solar flux that is externally incident on an opaque surface will be completely disregarded,

for example solar load on an opaque roof of a model whose internals only are modeled will not be

included as a heat gain. Instead, this heat gain should be manually calculated and applied as a

thermal condition, typically using a fixed heat flux or a radiation/mixed condition.

.... Using the Solar Load Model

When you want to run a steady-state solution with solar load enabled, you simply set up the solar

load model (Setting Up the Solar Load Model (p. )) and boundary conditions (Setting Boundary

Conditions for Solar Loading (p. )) for your case, and then run the simulation. The solution data

file will contain the solar fluxes that you can use for postprocessing. For a steady-state solution, the

solar loads are computed on initialization. If you want to initially solve a case without solar loading

(say, for stability) and then add the effects of solar loading afterward, you will need to enable the

solar load model through the text user interface (TUI).

Important

Note that you can compute the solar load at any time once you have set up the model by

using the sol-on-demand text interface command (see Additional Text Interface Com-

mands (p. ) for details).

When you want to run a transient solar load simulation, the process is the same as for the steady-

state case but you will need to specify the additional Time Steps per Solar Load Update parameter

in the Radiation Model dialog box. ANSYS Fluent will re-compute the sun position and irradiation

and update solar loads with this specified frequency.

Important

Note that parallel simulations involving the solar load model are set up and computed

using the same steps as in serial.

..... User-Defined Functions (UDFs) for Solar Load

You can write a user-defined function (UDF) to specify direct and diffuse solar intensity using the

DEFINE_SOLAR_INTENSITY macro. See DEFINE_SOLAR_INTENSITY for more information.

After it is interpreted or compiled, you can hook your intensity UDF for direct or diffuse solar irradi-

ation by selecting user-defined in the drop-down lists for these parameters in the Radiation

Model dialog box. See Step  in Setting Up the Solar Load Model (p. ) for details.

..... Setting Up the Solar Load Model

The solar load model is enabled in the Radiation Model dialog box (Figure . : The Radiation

Model Dialog Box (p. )).

Edit...

Figure . : The Radiation Model Dialog Box

Important

Solar load is available in the 3D solver only, and can be used to model steady and unsteady

flows.

The solar load model has two options: Solar Ray Tracing and Solar Irradiation. Solar Ray Tracing

can be applied as a stand-alone solar loading model, or it can be used in conjunction with one of

the ANSYS Fluent radiation models.Solar Irradiation is available only when the Discrete Ordinates

(DO) or Monte Carlo (MC)radiation model is enabled.

To set up the solar load model, perform the following steps:

. Enable the solar load model in the Radiation Model Dialog Box.

a.

To enable the solar ray tracing algorithm, select Solar Ray Tracing under Solar Load (Fig-

ure . :The Radiation Model Dialog Box (With Solar Load Model Solar Ray Tracing Option) (p. )).

Figure . : The Radiation Model Dialog Box (With Solar Load Model Solar Ray Tracing

Option)

b. To enable the Solar Irradiation option, first select the DO or MC model, and then select Solar Irradi-

Option)

ation under Solar Load (Figure . :The Radiation Model Dialog Box (with Solar Load Model Solar

Irradiation Option) (p. )).

Figure . : The Radiation Model Dialog Box (with Solar Load Model Solar Irradiation

Option)

. When using the non-gray DO or MC model, if the wavelengths of the specified bands do not cover the

entire solar spectrum, a message is written to the console displaying what percentage of the full solar

model has been covered. It is recommended that the full solar spectrum is considered.

When using the non-gray MC model, if you only specify one band then Fluent will automatically

cover the entire solar spectrum

. Define the solar parameters.

a.

Enter values for the X, Y, and Z components of the Sun Direction Vector. Alternatively, you can

choose to have this vector computed from the solar calculator by enabling the Use Direction

Computed from Solar Calculator option.

b. Specify the illumination parameters.

i.

Enter a value for Direct Solar Irradiation under Illumination Parameters.This parameter is

the amount of energy per unit area in

due to direct solar irradiation.This value may de-

pend on the time of year and the clearness of the sky. Make your selection in the drop-down list

next to Direct Solar Irradiation and either enter a constant value, have the value computed

from the solar calculator, or specify it using a user-defined function. (For more information

on writing solar intensity UDFs, see DEFINE_SOLAR_INTENSITY in the Fluent Customization

Manual.) For transient simulations, you have the additional option of specifying a time-dependent

piecewise-linear and polynomial profile for direct solar irradiation.

ii.

Enter a value for Diffuse Solar Irradiation for the DO model only, which is the amount of energy

per unit area in

due to diffuse solar irradiation.This value may depend on the time of

year, the clearness of the sky, and also on ground reflectivity. Make your selection in the drop-

down list next to Diffuse Solar Irradiation and either enter a constant value, have the value

computed from the solar calculator, or specify it using a user-defined function. (For more in-

formation on writing solar intensity UDFs, see DEFINE_SOLAR_INTENSITY in the .) For tran-

sient simulations, you have the additional option of specifying a time-dependent piecewise-

linear and polynomial profile for diffuse solar irradiation.

iii. If you are using the Solar Ray Tracing solar load model (Figure . :The Radiation Model

Dialog Box (With Solar Load Model Solar Ray Tracing Option) (p. )), then you will need to enter

a value for Spectral Fraction.The spectral fraction is the fraction of incident solar radiation in

the visible part of the solar radiation spectrum.

(.)

where

is the visible incident solar radiation, and

is the total incident solar radiation

(visible plus infrared).

. Use the solar calculator to compute solar beam direction and irradiation.

a.

Click Solar Calculator... in the Radiation Model dialog box to open the Solar Calculator dialog

box (Figure . :The Solar Calculator Dialog Box (p. )).

a.

Figure . : The Solar Calculator Dialog Box

b. In the Solar Calculator dialog box, define the Global Position by the following parameters:

i.

Enter a real number in degrees for Longitude.Values may range from

to

where neg-

ative values indicate the Western hemisphere and positive values indicate the Eastern hemisphere.

ii.

Enter a real number for Latitude in degrees.Values can range from

(the South Pole) to

(the North Pole), with

defined as the equator.

iii. Enter an integer for Timezone that is the local time zone in hours relative to Greenwich Mean

Time (+-GMT).This value can range from

to

.

Important

Note that you must specify all three Global Position parameters for the solar cal-

culator.

c.

Define the local Date and Time by the following parameters:

i.

Enter an integer for Day and Month under Day of Year.

ii.

Enter an integer for Hour that ranges from  to

under Time of Day. Enter an integer or

floating point number for Minute.

The time of day is based on a -hour clock:

hours and  minutes corresponds to :

a.m. and

hours

min corresponds to :. p.m. For example, if the local time

was :: a.m., you would enter  for Hour and . for Minute. If the local time was

: p.m., you would enter  for Hour and  for Minute.

d. Define the Mesh Orientation as the vectors for North and East in the CFD mesh system of coordinates.

e. Select the appropriate Solar Irradiation Method.The Fair Weather Conditions is the default

method.

f.

Enter an integer for Sunshine Fraction (default = ).

g. Click Apply.

method.

f.

The solar calculator output parameters are computed and the results are reported in the

console. The default values are shown below:

Fair Weather Conditions:

Sun Direction Vector: X: -., Y: ., X: .

Sunshine Fraction:

Direct Normal Solar Irradiation (at Earth’s surface) [W/m^]:

.

Diffuse Solar Irradiation - vertical surface: [W/m^]:

.

Diffuse Solar Irradiation - horizontal surface: [W/m^]:

.

Ground Reflected Solar Irradiation - vertical surface: [W/m^]:

.

. For transient simulations, enter the Time Steps Per Solar Load Update under Update Parameters.

The number of time steps that you specify will direct the ANSYS Fluent solver to update the solar load

data for the specified flow-time intervals in the unsteady solution process.

..... Setting Boundary Conditions for Solar Loading

Once you have defined the solar parameters for the solar load model (Setting Up the Solar Load

Model (p. )), you will need to set up boundary conditions for boundary zones that will participate

in solar loading. The boundary condition dialog boxes can be opened by right-clicking the boundary

name in the tree (under Setup/Boundary Conditions) and clicking Edit... in the menu that opens;

alternatively, you can open them from the Boundary Conditions task page:

Setup →

..... Solar Ray Tracing

Note

Solar ray tracing is designed to be applied to your geometrical information, therefore,

you must include every side of the external, or outer, enclosure/boundary for ray-tracing

Note

purposes, unless you expect that solar irradiation cannot enter through such boundaries.

If you exclude any internal zone from the solar load computation, then this would mean

that the resulting obstruction or blockage has been removed which would also be equi-

valent to a transparent surface. Excluded walls will also not participate in the computation

of scattered energy by the solar load model and, therefore, do not gain any heat from

scattered energy.

. Set the boundary condition for each inlet and exit boundary zone that you want to include in solar

loading.

a.

Open the inlet or exit boundary condition dialog box (for example, Velocity Inlet) and click the

Radiation tab (Figure . :The Velocity Inlet Dialog Box (p. )).

b. Enable the Participates in Solar Ray Tracing option (this option is enabled for all boundary condi-

tions by default). If you deactivate solar ray tracing by disabling this option the surface will be ignored

and the solar ray will pass through it with no interaction, regardless of the boundary condition type.

c.

Enter a value between  and  for the Solar Transmissivity Factor.This will allow you to control

the amount of solar irradiation entering the domain. By reducing the solar transmissivity factor from

to ., you can effectively cut the total internal energy source entering the domain by half.

Important

Note that the solar transmissivity factor is applied to both direct and diffuse solar

irradiation components.

d. Click OK.

Important

. Set the boundary condition for each wall boundary zone that you want to include in solar loading.

a.

Open a Wall boundary condition dialog box and click the Radiation tab.

b. Define the wall as opaque or semi-transparent. (An opaque wall will not allow any solar radiation

to pass through it, while a semi-transparent surface will allow a portion of the solar radiation to pass

through it.)

i.

For an opaque wall, select opaque from the drop-down list for BC Type (Figure . :The Wall

Dialog Box (p. )).Then enable the Participates in Solar Ray Tracing option (this option is

enabled for all boundary conditions by default) in the Solar Boundary Conditions group box

and enter constant values for Direct Visible and Direct IR absorptivity. Note that if you deactivate

solar ray tracing by disabling the Participates in Solar Ray Tracing option, the surface will be

ignored and the solar ray will pass through it with no interaction, regardless of the boundary

condition type.

Important

Absorption in the visible and infrared portions of the spectrum define the sur-

face material for the opaque wall.

ii.

For a semi-transparent wall, select semi-transparent from the drop-down list for BC Type (Fig-

ure . :The Wall Dialog Box (p. )).Then, enable the Participates in Solar Ray Tracing option

(this option is enabled for all boundary conditions by default) in the Solar Boundary Conditions

group box and enter constant values for Direct Visible, Direct IR, and Diffuse Hemispherical

absorptivity and transmissivity. Note that if you deactivate solar ray tracing by disabling the

Participates in Solar Ray Tracing option, the surface will be ignored and the solar ray will pass

through it with no interaction, regardless of the boundary condition type.

Important

For semitransparent coupled walls, the solar ray tracing settings are defined

on the original wall and not on the shadow wall.

Absorption and transmittance in the visible and infrared portions of the spectrum, as well

as the “shading” formulation (Diffuse Hemispherical), define the surface material for a

semi-transparent wall. These parameters are properties of the glazed unit and should be

provided by the glazing manufacturer. The direct components are based on normal incident

radiation (ANSYS Fluent adjusts this for the actual angle of incidence). Most manufacturers

present this information in a slightly different way so it may be necessary to seek guidance

from the supplier. Another useful source of data can be found in the ASHRAE Fundamentals

Handbook, chapter on Fenestration.

iii. Click OK.

Important

ANSYS Fluent will calculate the reflectivity as the difference between one and the sum

of absorptivity and transmissivity:

(.)

. Set the boundary condition for each porous jump boundary zone that you want to include in solar

loading.You can define the boundary such that it acts as a semi-transparent surface that will allow a

portion of the solar radiation to pass through it, along with fluid flow. In this way you can represent a

partial opening (for example, a grate, a grill, or a louver) that is a combination of gaps and (typically)

opaque surfaces.

a.

Open the Porous Jump boundary condition dialog box (Figure . :The Porous Jump Dialog

Box (p. )).

b. Define the Face Permeability, Porous Medium Thickness, Pressure-Jump Coefficient, and Thermal

Contact Resistance as described in User Inputs for the Porous Jump Model (p. ).

c.

Define the settings in the Solar Boundary Conditions group box.

i.

Enable the Participates in Solar Ray Tracing option (this option is enabled for all boundary

conditions by default). Note that if you deactivate solar ray tracing by disabling the Participates

in Solar Ray Tracing option, the surface will be ignored and the solar ray will pass through it

with no interaction, regardless of the boundary condition type.

ii.

Enter constant values (between  and ) for Direct Visible and Direct IR in the Absorptivity

group box.These values act as multipliers for the visible and infrared portions of the direct solar

radiation spectrum, respectively, to account for the absorption of the porous jump.

Important

One reasonable way to estimate the Direct Visible and Direct IR absorptivity

values for a grill, and so on, is to use the product of the obstructed area fraction

and the surface absorptivity. For example, if % of the grill facial area is ob-

structed with grill slats, and the slats have a surface absorptivity of ., you

could estimate the absorptivity as being ..

iii. Enter constant values (between  and ) for Direct Visible and Direct IR in the Transmissivity

radiation spectrum, respectively, to account for the transmissivity of the porous jump.

Important

One reasonable way to estimate the Direct Visible and Direct IR transmissivity

values for a grill, and so on, is to use the open area fraction. For example, if a

grill has openings between the slats that amount to % of the area, you could

estimate the transmissivity as being ..

..... Solar Irradiation

. For Solar Irradiation, all boundary conditions are set up as normal for the DO or MC model, except that

now you can select semi-transparent boundary surfaces that will provide a source of solar irradiation.

a.

Open a Wall boundary condition dialog box and click the Radiation tab (Figure . :The Wall

Dialog Box Radiation tab with Solar Irradiation (p. )).

Figure . : The Wall Dialog Box Radiation tab with Solar Irradiation

b. Select semi-transparent from the drop-down list for BC Type.

c.

Enable the Use Beam Direction from Solar Load Model Settings option, under Solar BC Options,

to have the values for beam direction applied from the Solar Load Model settings in the Radiation

Important

Note that the sign of the beam direction that is needed for the DO or MC model

is opposite the sun direction vector that is entered or derived from the solar

parameters. The beam direction in the DO or MC model is the direction of external

radiation (for example, radiation coming from the sun), while the sun direction

vector in the solar load model points to the sun.

d. Enable the Use Irradiation from Solar Load Model Settings option to have the irradiation specified

on the Radiation Model dialog box for the Solar Load model applied for direct and diffuse irradiation.

If selected while using the multiband approach for the DO or MC models, the direct and diffuse

(for DO only) irradiation is calculated and applied in each band, according to the black body

emission weighting factor.

When Use Irradiation from Solar Load Model Settings is enabled, the beam width will

automatically be set to

degrees - the angle subtended by the sun.

e. Click OK.

.....Text Interface-Only Commands

ANSYS Fluent has provided some additional commands for solar load setup that are only available

in the text interface. These commands are present in the following sections.

...... Automatically Saving Solar Ray Tracing Data

It is possible to direct ANSYS Fluent to automatically save solar load data to a generic file that you

can examine or use in an external program. This is done by executing the text command autosave-

solar-data from the text interface.

define → models → radiation → solar-parameters → autosave-solar-data

. Enter a value for the autosave solar data file frequency when prompted, in order to specify the frequency

(in time steps) at which you want the solar load data written to a file.The default value is zero, which

means that no automatic saving is performed.

. Enter the filename, in quotations.

. Choose to write file in binary format.

The text interface command for autosave-solar-data for a file named solar and a frequency

of  is shown below:

/define/models/radiation/solar-parameters> autosave-solar-data

Autosave Solar Data File Frequency []

Enter Filename [""] "solar"

...... Automatically Reading Solar Data

When you are executing a transient simulation in serial or parallel ANSYS Fluent  version . or later

and you want to read the solar load data file from a serial run performed in an earlier version, you

can use the following text command:

define → models → radiation → solar-parameters → autoread-solar-data

. Enter a value for the autoread solar data file frequency when prompted, in order to specify the frequency

(in time steps) at which you want the solar load data read from the file generated during the serial run.

The default value is zero, which means that no automatic reading is performed.

The text interface command for autoread-solar-data for a file named solar and a frequency

/define/models/radiation/solar-parameters> autoread-solar-data

Autoread Solar Data File Frequency []

Use Binary Format for Reading Data Files [yes]

...... Aligning the Camera Direction With the Position of the Sun

When the solar load model is enabled, you can direct ANSYS Fluent to align the camera direction

with the sun position using the text interface command:

define → models → radiation → solar-parameters → sol-camera-pos

This command is useful when you are executing a transient simulation and you want to capture an

image of your model with solar load parameters displayed (such as solar heat flux) as the sun position

changes with time in order to create an animation. See Postprocessing Solar Load Quantities (p. )

...... Specifying the Scattering Fraction

You can modify the default scattering fraction ( ) using the text interface command:

The scattering fraction is the amount of direct radiation that has been reflected from opaque surfaces

(after entering through the transparent surfaces) that will be considered to remain within the space

and be evenly distributed among all surfaces. The value is between  and .

The text interface command for specifying a scattering-fraction of

is shown below:

/define/models/radiation/solar-parameters> scattering-fraction

Scattering Fraction [] .

...... Applying the Solar Load on Adjacent Fluid Cells

You can direct ANSYS Fluent to apply the solar load that is computed from the solar ray tracing al-

gorithm to adjacent fluid cells by issuing the following command at the text interface:

define → models → radiation → solar-parameters → sol-adjacent-fluidcells

The text interface command is shown below:

/define/models/radiation/solar-parameters> sol-adjacent-fluidcells

Apply Solar Load on adjacent Fluid Cells? [no] y

This command allows you to apply solar loads to adjacent fluid cells only, even if solid or shell con-

duction zones are present. By applying the solar load on adjacent fluid cells, you are overruling the

default order of the adjacent cell assignment in ANSYS Fluent which is shell, solid, fluid.

...... Specifying Quad Tree Refinement Factor

You can modify the default value ( ) for the maximum quad tree refinement factor in the solar ray

tracing algorithm using the text command:

define → models → radiation → solar-parameters → quad-tree-parameters

The text interface command is shown below, when a new maximum refinement value of

is spe-

cified:

/define/models/radiation/solar-parameters> quad-tree-parameters

Maximum Quad-Tree Refinement []

...... Specifying Ground Reflectivity

You can modify the default value (

) for the ground reflectivity using the text command:

Ground reflectivity

(Equation . (p. )) includes the contribution of reflected solar radiation

from ground surfaces. It is treated as part of the total diffuse solar irradiation when the solar calcu-

lator is used in conjunction with the Diffuse Solar Irradiation illumination parameter.

The default value is

.

/define/models/radiation/solar-parameters> ground-reflectivity

Ground Reflectivity [.] .

...... Reverting to Single Band Implementation of DO Model

For consistency with cases set up previous to Fluent  r1, you can use the following command

so that the complete solar load is applied to the first band only.

define → models → radiation → apply-full-solar-irradiation?

/define/models/radiation/apply-full-solar-irradiation?

Apply full solar irradiation to first band? [no] yes

...... Additional Text Interface Commands

Some solar load commands that are available in the graphical user interface are also made available

in the text interface. For example, you can turn the solar load model on using the text command:

define → models → radiation → solar?

You can also enter the solar calculator parameters in the text interface by executing the command:

define → models → radiation → solar-calculator

Once invoked, you will be prompted to enter the solar calculator input parameters.

To set the illumination parameters, select this option from the solar-parameters menu:

define → models → radiation → solar-parameters → illumination-parameters

And finally, you can direct ANSYS Fluent to compute the solar load on demand, by issuing the text

command:

define → models → radiation → solar-parameters → sol-on-demand

When the command is initiated, the solar data are written to the console.

.... Postprocessing Solar Load Quantities

The following solar load quantities can be used to visualize the illuminated areas and shadows created

by solar radiation.

solar heat flux (that is, sum of visible and IR absorbed solar flux on opaque walls)

absorbed visible and IR solar flux (semi-transparent walls and porous jump boundaries only)

reflected visible and IR solar flux (semi-transparent walls and porous jump boundaries only)

transmitted visible and IR solar flux (semi-transparent walls and porous jump boundaries only)

These quantities are available for postprocessing of solar loading at wall boundaries and can be dis-

played as contours of Wall Fluxes in the Contours dialog box. For steady-state simulations, the solar

flux data is computed at solution initialization and is available for postprocessing. You can also compute

the solar load at any time during your ANSYS Fluent session, after you have set up the model and

applied boundary conditions. To compute the solar load on demand, you can issue the sol-on-

demand command in the text interface (see Additional Text Interface Commands (p. ) for details).

Solar heat flux, for example, can be displayed for surfaces using the Contours dialog box. A sample

dialog box is shown below (Figure . : The Contours Dialog Box (p. )).

Results → Graphics → Contours

New...

Figure . : The Contours Dialog Box

..... Solar Load Animation at Different Sun Positions

The solar camera alignment command is useful when you want to take timed pictures of solar

loading effects of your model during transient simulations, and later create animations of the image

files using an external program. Follow the procedure below.

. Read (or set up) your transient case file in ANSYS Fluent.

. Set up the automatic execution of solution commands in the Execute Commands dialog box that will:

) display solar load parameter graphics, ) re-position the solar camera such that the view is aligned

with the instantaneous sun direction, and ) generate a picture image file (.tiff) during the solution

process in the Execute Commands dialog box.

Edit...

. Initialize and run the solution.

. Animate the .tiff files using an external animation tool.

The following commands entered in the Execute Commands dialog box will direct ANSYS Fluent to

display contours of solar heat flux, align the camera with the current direction of the sun, and then

generate a picture image file (.tiff) of the solar heat flux contour every  time steps during the

unsteady simulation. See Figure . : The Execute Commands Dialog Box (p. ).

/di/cont solar-heat-flux ,,

/def/mod/rad/solar-para/sol-camera-pos

/di/hc "flux-%t.tiff"

Figure . : The Execute Commands Dialog Box

..... Reporting and Displaying Solar Load Quantities

ANSYS Fluent provides some additional solar load variables that you can use for postprocessing

when your model includes solar ray tracing. You can generate graphical plots or alphanumeric reports

of the following variables:

Transmitted Visible Solar Flux (semi-transparent walls and porous jump boundaries)

Transmitted IR Solar Flux (semi-transparent walls and porous jump boundaries)

Reflected Visible Solar Flux (semi-transparent walls and porous jump boundaries)

Reflected IR Solar Flux (semi-transparent walls and porous jump boundaries)

Absorbed Visible Solar Flux (semi-transparent walls and porous jump boundaries)

Absorbed IR Solar Flux (semi-transparent walls and porous jump boundaries)

See Field Function Definitions (p. ) for their definitions.

ANSYS Fluent is able to predict heat transfer in periodically repeating geometries, such as compact heat

exchangers, by including only a single periodic module for analysis.

This section discusses streamwise-periodic heat transfer. The treatment of streamwise-periodic flows is

discussed in Periodic Flows (p. ), and a description of no-pressure-drop periodic flow is provided in

Periodic Boundary Conditions (p. ).

Information about streamwise-periodic heat transfer is presented in the following sections:

...Theory

... Using Periodic Heat Transfer

... Solution Strategies for Periodic Heat Transfer

... Monitoring Convergence

... Postprocessing for Periodic Heat Transfer

The following sections contain information about periodic heat transfer:

.... Constraints for Periodic Heat Transfer Predictions

As discussed in Overview and Limitations (p. ), streamwise-periodic flow conditions exist when the

flow pattern repeats over some length , with a constant pressure drop across each repeating module

along the streamwise direction.

Periodic thermal conditions may be established when the thermal boundary conditions are of the

constant wall temperature or wall heat flux type. In such problems, the temperature field (when scaled

in an appropriate manner) is periodically fully developed  [] (p. ). As for periodic flows, such

problems can be analyzed by restricting the numerical model to a single module or periodic length.

In addition to the constraints for streamwise-periodic flow discussed in Limitations for Modeling

Streamwise-Periodic Flow (p. ), the following constraints must be met when periodic heat transfer

is to be considered:

The pressure-based solver must be used.

The thermal boundary conditions must be of the specified heat flux or constant wall temperature type.

Furthermore, in a given problem, these thermal boundary types cannot be combined: all boundaries must

be either constant temperature or specified heat flux.You can, however, include constant-temperature

walls and zero-heat-flux walls in the same problem. For the constant-temperature case, all walls must be

at the same temperature (profiles are not allowed) or zero heat flux. For the heat flux case, profiles and/or

different values of heat flux may be specified at different walls.

When constant-temperature wall boundaries are used, you cannot include viscous heating effects or any

volumetric heat sources.

Modeling Periodic Heat Transfer

In cases that involve solid regions, the regions cannot straddle the periodic plane.

The thermodynamic and transport properties of the fluid (heat capacity, thermal conductivity, viscosity,

and density) cannot be functions of temperature. (You cannot, therefore, model reacting flows.) Transport

properties may, however, vary spatially in a periodic manner, and this allows you to model periodic turbulent

flows in which the effective turbulent transport properties (effective conductivity, effective viscosity) vary

with the (periodic) turbulence field.

Theory (p. ) and  Using Periodic Heat Transfer (p. ) provide more detailed descriptions of the

input requirements for periodic heat transfer.

...Theory

...Theory

Streamwise-periodic flow with heat transfer from constant-temperature walls is one of two classes of

periodic heat transfer that can be modeled by ANSYS Fluent. A periodic fully developed temperature

field can also be obtained when heat flux conditions are specified. In such cases, the temperature

change between periodic boundaries becomes constant and can be related to the net heat addition

from the boundaries as described in this section.

Important

Periodic heat transfer can be modeled only if you are using the pressure-based solver.

.... Definition of the Periodic Temperature for Constant- Temperature Wall

Conditions

For the case of constant wall temperature, as the fluid flows through the periodic domain, its temper-

ature approaches that of the wall boundaries. However, the temperature can be scaled in such a way

that it behaves in a periodic manner. A suitable scaling of the temperature for periodic flows with

constant-temperature walls is  [] (p. )

(.)

The bulk temperature,

, is defined by

(.)

where the integral is taken over the inlet periodic boundary ( ). It is the scaled temperature,

, which

obeys a periodic condition across the domain of length .

.... Definition of the Periodic Temperature Change σ for Specified Heat Flux

When periodic heat transfer with heat flux conditions is considered, the form of the unscaled temper-

ature field becomes analogous to that of the pressure field in a periodic flow:

(.)

where  is the periodic length vector of the domain. This temperature gradient,

, can be written in

(.)

terms of the total heat addition within the domain,

, as

(.)

where

is the specified or calculated mass flow rate.

A typical calculation involving both streamwise-periodic flow and periodic heat transfer is performed

in two parts. First, the periodic velocity field is calculated (to convergence) without consideration of

the temperature field. Next, the velocity field is frozen and the resulting temperature field is calculated.

These periodic flow calculations are accomplished using the following procedure:

. Set up a mesh with translationally periodic boundary conditions.

. Specify constant thermodynamic and molecular transport properties.

. Specify either the periodic pressure gradient or the net mass flow rate through the periodic boundaries.

. Compute the periodic flow field, solving momentum, continuity, and (optionally) turbulence equations.

. Specify the thermal boundary conditions at walls as either heat flux or constant temperature.

. Define an inlet bulk temperature.

. Solve the energy equation (only) to predict the periodic temperature field.

In order to model the periodic heat transfer, you will need to set up your periodic model in the manner

described in User Inputs for the Pressure-Based Solver (p. ) for periodic flow models with the pressure-

based solver, noting the restrictions discussed in Limitations for Modeling Streamwise-Periodic

Flow (p. ) and Constraints for Periodic Heat Transfer Predictions (p. ). In addition, you will need

to provide the following inputs related to the heat transfer model:

. Enable the solution of the energy equation by right-clicking Energy in the tree (under Setup/Models)

and clicking On in the menu that opens (Figure . : Enabling the Energy Equation (p. )).

On

. Define the thermal boundary conditions according to one of the following procedures.The boundary

condition dialog boxes can be opened by right-clicking the boundary name in the tree (under

Setup/Boundary Conditions) and clicking Edit... in the menu that opens; alternatively, you can open

them from the Boundary Conditions task page:

Setup →

If you are modeling periodic heat transfer with specified-temperature boundary conditions, set the wall

for all wall boundaries in their respective Wall dialog box. Note that all wall bound-

aries must be assigned the same temperature and that the entire domain (except the periodic bound-

aries) must be “enclosed” by this fixed-temperature condition, or by symmetry or adiabatic ( =)

If you are modeling periodic heat transfer with specified-heat-flux boundary conditions, set the wall

heat flux in the Wall dialog box for each wall boundary.You can define different values of heat flux on

different wall boundaries, but you should have no other types of thermal boundary conditions active

in the domain.

. Define solid regions, if appropriate, according to one of the following procedures.The cell zones can be

defined by right-clicking the zone name in the tree (under Setup/Cell Zone Conditions), or using the

Cell Zone Conditions task page:

Setup →

Setup →

If you are modeling periodic heat transfer with specified-temperature conditions, conducting solid regions

can be used within the domain, provided that on the perimeter of the domain they are enclosed by

the fixed-temperature condition. Heat generation within the solid regions is not allowed when you are

solving periodic heat transfer with fixed-temperature conditions.

If you are modeling periodic heat transfer with specified-heat-flux conditions, you can define conducting

solid regions at any location within the domain, including volumetric heat addition within the solid, if

desired.

. Set constant material properties (density, heat capacity, viscosity, thermal conductivity), not temperature-

dependent properties, using the Create/Edit Materials dialog box.This dialog box can be opened by

right-clicking the material name in the tree (under Setup/Materials) and clicking Edit... in the menu that

opens; alternatively, you can open them from the Materials task page:

Setup →

Materials

. Specify the Upstream Bulk Temperature in the Periodic Conditions dialog box, which can be opened

from Boundary Conditions task page:

Setup →

Important

If you are modeling periodic heat transfer with specified-temperature conditions, the

bulk temperature should not be equal to the wall temperature, since this will give you

the trivial solution of constant temperature everywhere.

. Set the solution parameters as described in Solution Strategies for Periodic Heat Transfer (p. ).

. Run the solution and monitor the convergence as described in Monitoring Convergence (p. ).

. Postprocess the results as described in Postprocessing for Periodic Heat Transfer (p. ).

After completing the inputs described in Using Periodic Heat Transfer (p. ), you can solve the flow

and heat transfer problem to convergence. The most efficient approach to the solution, however, is a

sequential one in which the periodic flow is first solved without heat transfer and then the heat

transfer is solved leaving the flow field unaltered. This sequential approach is accomplished as follows:

. Disable solution of the energy equation in the Equations dialog box; this dialog box is accessed by right-

clicking Solution Controls in the tree (under Solution) and clicking Equations... in the menu that opens.

. Solve the remaining equations (continuity, momentum, and, optionally, turbulence parameters) to con-

vergence to obtain the periodic flow field.

Important

When you initialize the flow field before beginning the calculation, use the mean value

between the inlet bulk temperature and the wall temperature for the initialization of

the temperature field.

. Return to the Equations dialog box and turn off solution of the flow equations and turn on the energy

solution.

. Solve the energy equation to convergence to obtain the periodic temperature field of interest.

While you can solve your periodic flow and heat transfer problems by considering both the flow and

heat transfer simultaneously, you will find that the procedure outlined above is more efficient.

If you are modeling periodic heat transfer with specified-temperature conditions, you can monitor the

value of the bulk temperature ratio

(.)

during the calculation by creating a report plot that includes bulk temperature ratio (periodic-bulk-

temperature-ratio), to ensure that you reach a converged solution. See Monitoring Statistics (p. )

for additional information.

The actual temperature field predicted by ANSYS Fluent in periodic models will not be periodic, and

viewing the temperature results during postprocessing will display this actual temperature field (

of Equation . (p. )). The displayed temperature may exhibit values outside the range defined

by the inlet bulk temperature and the wall temperature. This is permissible since the actual temperature

profile at the inlet periodic face will have temperatures that are higher or lower than the inlet bulk

Static Temperature is found in the Temperature... category of the variable selection drop-down

list that appears in postprocessing dialog boxes.

Figure . : Temperature Field in a 2D Heat Exchanger Geometry With Fixed Temperature Boundary

Conditions (p. ) shows the temperature field in a periodic heat exchanger geometry.

Figure . : Temperature Field in a 2D Heat Exchanger Geometry With Fixed Temperature

Chapter : Modeling Heat Exchangers

contain tubular heat exchangers. However, for most engineering problems, it is impractical to model

individual fins and tubes of a heat exchanger core. In principle, heat exchanger cores introduce a

pressure drop to the primary fluid stream and transfer heat from or to a second fluid (for example, a

coolant), referred to here as the auxiliary fluid.

ANSYS Fluent provides two distinct methods of modeling a heat exchanger: the dual cell model and

the macro model. These models can be used to compute the auxiliary fluid inlet temperature for a fixed

heat rejection or the total heat rejection for a fixed auxiliary fluid inlet temperature. The dual cell

model allows the solution of the passes of the auxiliary flow on a separate mesh, that is, other than the

primary fluid mesh (see Figure . : An Example of a Four-Pass Heat Exchanger (p. )), unlike the macro

model, where the auxiliary flow passes are modeled as 1D flow.

Figure . : An Example of a Four-Pass Heat Exchanger

Important

Note that the heat exchanger models are not appropriate for modeling a cold-only flow; in

such a case, you should instead use the porous media model, as described in Porous Media

Conditions (p. ).

For theoretical information about the various heat exchanger models, refer to Heat Exchangers in the

The following sections contain information about the heat exchanger models:

.. Choosing a Heat Exchanger Model

..The Dual Cell Model

..The Macro Heat Exchanger Models

.. Postprocessing for the Heat Exchanger Model

.. Useful Reporting TUI Commands

ANSYS Fluent provides various options for modeling heat exchangers, each with their own features and

limitations. The following instructions can help you determine which option/combination of options is

the most appropriate for your problem.

. Decide whether you want to use the dual cell model or the macro model.

a.

The dual cell model provides the greatest flexibility with regard to the shape of the heat exchanger

core and the nature of the mesh, and allows the auxiliary fluid to be highly non-uniform as it enters

the core (for example, due to passing through arbitrary shaped inlet tanks). However, the dual cell

model may need to be discounted as an option because of the following limitations:

If the heat exchanger performance data that you have is in the form of a velocity vs. effectiveness

curve, the dual cell model cannot be used.

The dual cell model does not allow you to model phase change in the auxiliary fluid.

If the previous limitations are not relevant for your problem, you can proceed directly to using

the dual cell model, as described in Using the Dual Cell Heat Exchanger Model (p. ).

b. While the macro model has more restrictions than the dual cell model, it is quite suitable for a thin 3D

heat exchanger core with a rectangular cross-section, where the pass-to-pass plane is perpendicular

to the primary flow direction, the auxiliary flow is uniform (so it can be treated as a 1D flow), and the

mesh is uniform and structured.To verify that your problem can tolerate the limitations of the macro

model, see Restrictions (p. ).

. If you chose to use the macro model in the previous step, you must decide whether you want to use the

grouped or ungrouped version of this model. If you want to define a single heat exchanger using multiple

fluid zones, or if you would like to connect the fluid flow path among multiple heat exchangers, you should

use the grouped version, as described in Using the Grouped Macro Heat Exchanger Model (p. ). Otherwise,

you can use the ungrouped version, as described in Using the Ungrouped Macro Heat Exchanger Mod-

el (p. ).

. If you chose to use the macro model in the step ., you must decide whether you want to model the heat

transfer using the number-of-transfer-units (NTU) method or the simple effectiveness method.This decision

largely rests on the kind of experimental data that you have: the NTU method requires that you provide

the various primary fluid flow rates and auxiliary fluid flow rates and the corresponding heat transfer values;

the simple effectiveness method requires that you provide the data points for a curve that defines how

the effectiveness (that is, the ratio of actual rate of heat transfer between the primary and auxiliary fluids

to the maximum possible rate of heat transfer) varies with the fluid velocity. Additionally, you should

Modeling Heat Exchangers

consider the differences between the two heat transfer models outlined in Table . : NTU Model Vs. Simple

Effectiveness Model (p. ).

Table . : NTU Model Vs. Simple Effectiveness Model

Simple Effectiveness

Model

NTU Model

single phase and two

Model

NTU Model

phase

single phase only

How many phases are allowed in the auxiliary flow?

No

Yes

Can you model primary fluid-side reverse flow?

No

Yes

Can the primary fluid have a variable density?

Yes

No

Must the primary fluid heat capacity be less than the

auxiliary fluid heat capacity?

You will specify whether you want the NTU or simple effectiveness model in the Model Data tab

of either the Ungrouped Macro Heat Exchanger dialog box or the Heat Exchanger Group dialog

box, depending on whether you opted for the ungrouped or grouped version of the macro model,

An overview of the options available to you when modeling heat exchangers is shown in Figure . : Heat

Exchanger Modeling Options (p. ).

Figure . : Heat Exchanger Modeling Options

The dual cell heat exchanger model allows the solution of both the primary and auxiliary flow on sep-

arate co-located meshes and couples the two flows only through heat transfer at the heat exchanger

core.

For theoretical information about this model, refer to The Dual Cell Model in the Theory Guide.

The Dual Cell Model

... Restrictions

The following restrictions exist for the dual cell heat exchanger models:

The simple effectiveness model is not available.

The heat exchanger performance data must be in the form of heat transfer rates or number of transfer

units (NTU) for auxiliary / primary fluid flow rate combinations, rather than a velocity vs. effectiveness curve.

In the case of a heat exchanger in which the primary and auxiliary meshes are not identical, heat transfer

may be non-conservative (that is, the heat lost by the hot fluid may not equal the heat gained by the cold

fluid).To minimize the difference in heat transfer, the topology and size of the primary and auxiliary cells

should be as similar as possible, with the ideal being one-to-one cell conductivity. Note that you can make

the meshes identical by copying a zone via the mesh/modify-zones/copy-move-cell-zone text

command.

... Using the Dual Cell Heat Exchanger Model

The steps for setting up the dual cell heat exchanger model is as follows:

. Read the mesh file.

a.

If the mesh file does not already contain overlapping heat exchanger cores for primary and auxiliary

fluids, then you must create a duplicate of the zone that represents the core using the following text

command:

See Copying Cell Zones (p. ) for details on copying meshes.

b. Make sure that the auxiliary fluid mesh is divided into separate zones, one for each pass.

See Separating Cell Zones (p. ) for details on separating meshes.

c.

Make sure that the inlet and outlet for the heat exchanger are two separate zones.

. Enable the calculation of energy in the Energy dialog box.

ON

. Enable the Dual Cell Model in the Heat Exchanger Model dialog box and click Define... (Figure . :The

Heat Exchanger Model Dialog Box (p. )).

Setup → Models → Heat Exchanger

Edit...

Figure . : The Heat Exchanger Model Dialog Box

. Specify the inputs to the dual cell heat exchanger model, using the Dual Cell Heat Exchanger dialog box

Edit...

(Figure . :The Dual Cell Heat Exchanger Dialog Box (p. )).

Figure . : The Dual Cell Heat Exchanger Dialog Box

. Click New... to define the heat exchanger.The Set Dual Cell Heat Exchanger dialog box will appear

(Figure . :The Set Dual Cell Heat Exchanger Dialog Box (p. )), where you will define the heat exchanger

Figure . : The Set Dual Cell Heat Exchanger Dialog Box

a.

Enter the heat exchanger Name or keep the default name.The suffix - is incremented automatically

on defining more than one heat exchanger.

b. In the Fluid Zones tab (Figure . :The Set Dual Cell Heat Exchanger Dialog Box (p. ))

i.

Specify the Number of Passes of your heat exchanger.

ii.

Select the appropriate Primary and Auxiliary Fluid Zone, representing the heat exchanger core.

Important

The selected zones must be overlapping in physical space.

c.

Click the Heat Rejection tab (Figure . :The Heat Rejection Tab (p. )).

Figure . : The Heat Rejection Tab

i.

If you select Fixed Heat Rejection, set the inputs for the following:

Heat Rejection Targeted which is the heat rejection desired from the heat exchanger.

Inlet Zone for Temperature Updates allows ANSYS Fluent to change the temperature of the

specified inlet zone in order to match the targeted heat rejection.

Temperature Update Under-Relaxation is a factor that controls convergence.

Iteration Interval Between Temperature Updates is used to control divergence.

ii.

Select Fixed Inlet Temperature if the output desired is total heat rejection.

ii.

d. Click the Performance Data tab (Figure . :The Performance Data Tab (p. )).

Figure . : The Performance Data Tab

You must decide whether you will select Raw Data or NTU Data from the Options list. Using

the Raw Data option specifies that the effectiveness ( ) is evaluated as the ratio of the rate of

heat transfer between the primary and auxiliary fluids (which you define in a table format) to

the maximum possible rate of heat transfer (

) for the current flow regime (see Equation .

in the Theory Guide). The calculated efficiency is then used to calculate the NTU value using

the crossflow formula for each and every set of primary and auxiliary flow rates.

If the heat exchanger manufacturer used a similar approach in evaluating the NTU values, then

there is no difference between the Raw Data and NTU Data options. However, if a different

methodology was used by the manufacturer that accounts for some possible non-uniformity

of the profile or for the partial mixing of the flow stream, then the NTU Data option is likely

to be more accurate. Similarly, you may be able to assess more accurate NTU values for your

case using tables from the relevant literature. This can even include some mixing of the oncoming

flow stream, for situations where the primary flow can deviate from the direction normal to the

heat exchanger tubes; this can happen in heat exchangers where the fins are either very spaced

or absent. Therefore, the NTU Data option can be more accurate if the NTU values are gathered

at non-ideal conditions that bear a close resemblance to your simulated scenario.

i.

i.

If you select the Raw Data option, then specify the following:

Heat Transfer Data... opens the Heat Transfer Data Table Dialog Box (p. ), where you will

enter experimental data that defines how heat transfer values relate to the fluid flow rates (Fig-

ure . :The Heat Transfer Data Table Dialog Box (p. )). See Specifying Heat Exchanger Per-

formance Data (p. ) more details.

Figure . : The Heat Transfer Data Table Dialog Box

Effectiveness-NTU Relation computes the NTU values from the heat transfer data. Choose

cross-flow-unmixed, parallel-flow, or counter-flow, all of which are described in NTU Relations.

Auxiliary Fluid Temperature is the inlet reference temperature for the auxiliary fluid.

Primary Fluid Temperature is the inlet reference temperature for the primary fluid.

ii.

If you select the NTU Data option, click NTU Table... to access the NTU Table dialog box. Populate

this table in the same manner as described previously for the Heat Transfer Data Table Dialog

Box (p. ). More information is available in Specifying Heat Exchanger Performance Data (p. ).

e. Click the Frontal Area tab.You have the option to specify the Primary and Auxiliary Fluid Core

Frontal Area directly, or compute the area from a surface zone, as shown in Figure . :The Frontal

Area Tab (p. ).

Figure . : The Frontal Area Tab

f.

Click the Coupling tab if you want to couple the heat exchanger passes (Figure . :The Coupling

Tab (p. )).

Figure . : The Coupling Tab

f.

Tab (p. )).

Consider the following example illustrating the coupling of a four-pass heat exchanger.

Figure . : An Example of a Four-Pass Heat Exchanger (p. ) shows a four-pass heat exchanger

with air as the primary fluid and the coolant as the auxiliary fluid. The coolant flows through

the tubes in a serpentine manner and air flows normal to the tubes, forming a cross flow pattern.

To model this type of flow using the dual cell heat exchanger model, you must first generate

the mesh. The mesh should contain the following:

i.

A single primary cell zone.

ii.

Four adjacent auxiliary cell zones, one for each pass. Each auxiliary zone should be separated from

the other by a coupled or uncoupled wall. Each pass will have its own inlet and outlet zones.

iii. The primary and four auxiliary zones should overlap in physical space.

In the Coupling tab, mass-weighted-average is selected by default for the Temperature of

the outlet of Pass  to the inlet of Pass . Similarly, the mass-weighted-average temperature of

the outlet of Pass  will be applied at the inlet zone of Pass , and so on. Alternatively, you can

couple the passes by using Profiles... in the Boundary Conditions task page or by using user-

defined functions to define the Temperature in the Thermal tab of the relevant boundary

condition dialog boxes. If you do so, make sure you select none from the Temperature drop-

down list in the Coupling tab of the Set Dual Heat Exchanger dialog box.

Important

Important

Make sure to specify the auxiliary zones in the correct order (that is the zone for Pass

should be selected first, then Pass , and so on) in the Fluid Zones tab of the Set

Dual Cell Heat Exchanger dialog box.

g. Click Apply to save the heat exchanger inputs.

. To view the plot of NTU vs. primary mass flow rate for each auxiliary mass flow rate, click Plot NTU.

The Plot NTU button will plot the performance data curve for the selected heat exchanger. The

performance data is supplied through the Performance Data tab.

When you close the Set Dual Cell Heat Exchanger dialog box, you will return to the Dual Cell

Heat Exchanger dialog box, where you should now see the heat exchanger name in the Heat

Exchanger list.

You can

Modify the settings of heat exchanger by selecting it from the list and clicking Modify....

Copy the data of one heat exchanger to another using the Copy button, assuming you have more than

one heat exchanger.

Delete any unwanted heat exchangers by selecting the heat exchanger from the list and clicking Delete.

Important

All the inputs are copied except for the name, primary fluid zone and auxiliary fluid

zone.

To use the macro heat exchanger model, you must define one or more fluid zone(s) to represent the

heat exchanger core. Typically, the fluid zone is sized to the dimension of the core itself. As part of the

setup procedure, you will define the auxiliary fluid path, the number of macros, and the physical prop-

erties and operating conditions of the core (pressure drop parameters, heat exchanger effectiveness,

auxiliary fluid flow rate, and so on).

Additional information about macro heat exchangers can be found in Overview of the Macro Heat Ex-

changer Models in the Theory Guide. For the theory behind these models, refer to Macro Heat Exchanger

Model Theory in the Theory Guide.

ANSYS Fluent provides two heat transfer models: the default NTU model and the simple effectiveness

model. The simple effectiveness model interpolates the effectiveness from the velocity vs. effectiveness

curve that you provide. For the NTU model, ANSYS Fluent calculates the effectiveness, , from the NTU

value that is calculated by ANSYS Fluent from the heat transfer data provided by you in tabular format.

ANSYS Fluent will automatically convert this heat transfer data to a primary fluid mass flow rate vs. NTU

curve (this curve will be piecewise linear). This curve will be used by ANSYS Fluent to calculate the NTU

for macros based on their size and primary fluid flow rate.

The NTU model provides the following features:

The model can be used to check heat capacity for both the primary and the auxiliary fluid and takes the

lesser of the two for the calculation of heat transfer.

The model can be used to model heat transfer to the primary fluid from the auxiliary fluid, and vice versa.

The model can be used to model primary fluid-side reverse flow.

The model can be used with variable density of the primary fluid.

The model can be used in either the serial or parallel ANSYS Fluent solvers.

The model can be used to make a network of heat exchangers using a heat exchanger group (Using the

Grouped Macro Heat Exchanger Model (p. )).

Transient profiles can be used for the auxiliary fluid inlet temperature and for total heat rejection.

Transient profiles can be used for auxiliary mass flow rates.

The simple effectiveness model provides the following features:

The model can be used to model heat transfer from the auxiliary fluid to the primary fluid, and vice versa.

The auxiliary fluid properties can be a function of pressure and temperature, therefore allowing phase change

of the auxiliary fluid.

The model can be used by serial as well as parallel solvers.

The Macro Heat Exchanger Models

... Using the Ungrouped Macro Heat Exchanger Model

... Using the Grouped Macro Heat Exchanger Model

The following restrictions exist for the macro heat exchanger models:

The core must be a 3D mesh with a cross-section that is approximately rectangular in shape.

The primary fluid streamwise direction (see Equation . in the Theory Guide) must be aligned with one

of the three orthogonal axes defined by the rectangular core.

The pass-to-pass plane must be perpendicular to the primary fluid streamwise direction.

The two dimensions of the pass-to-pass plane can each be discretized into multiple macroscopic cells

(macros), but in the direction perpendicular to this plane the macros cannot be subdivided.

It is highly recommended that the free-form Tet mesh is not used in the macro heat exchanger model. In-

stead, evenly distributed Hex/Wedge cells should be used for improved accuracy and a more robust

solution process.

Flow acceleration effects are neglected in calculating the pressure loss coefficient.

For the simple effectiveness model, the primary fluid must have a capacity rate that is less than that of the

auxiliary fluid.

Auxiliary fluid phase change cannot be modeled using the NTU model.

The macro-based method requires that an equal number of cells reside in each macro of equal size and

shape.

The auxiliary fluid flow is assumed to be 1D.

The pass width has to be uniform.

Accuracy is not guaranteed when the mesh is not structured or layered.

Accuracy is not guaranteed when there is upstream diffusion of temperature at the inlet/outlet of the core.

Non-conformal meshes cannot be attached to the inlet/outlet of the core. An extra layer has to be created

to avoid it.

The heat exchanger model settings may be written into and read from the boundary conditions file

(Reading and Writing Boundary Conditions (p. )) using the text commands, file/write-settings

and file/read-settings, respectively. Otherwise, the steps for setting up the ungrouped macro

heat exchanger model is as follows:

. Read the mesh and make sure that the inlet and outlet for the heat exchanger are two separate zones.

. Enable the calculation of energy in the Energy Dialog Box (p. ).

ON

. Enable the Ungrouped Macro Model option and click the Define... button in the Heat Exchanger Model

Dialog Box (p. ) (Figure . :The Heat Exchanger Model Dialog Box (p. )) to access the Ungrouped

Macro Heat Exchanger dialog box.

Edit...

. Specify the heat exchanger inputs in the Ungrouped Macro Heat Exchanger dialog box.

Figure . : The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Model Data

Tab

a.

In the Fluid Zone drop-down list, select the fluid zone representing the heat exchanger core.

b. Under the Model Data tab, choose Fixed Heat Rejection or Fixed Inlet Temperature, as required

(Figure . :The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Model Data Tab (p. )).

c.

Specify the Heat Transfer Model as either the default ntu-model or the simple-effectiveness-

model. See step  in Choosing a Heat Exchanger Model (p. ) for details about the differences between

these two models.

d. Specify the Core Porosity Model if you want ANSYS Fluent to use the pressure loss coefficient function

to automatically compute (and update) the porous media coefficients in the cell zones condition dialog

box, as described in Streamwise Pressure Drop in the Theory Guide. More information is available in

Setting the Pressure-Drop Parameters and Effectiveness (p. ).

e. If the ntu-model is chosen, a Heat Transfer Data... button will appear under Heat Exchanger Per-

formance Data. Clicking the Heat Transfer Data... button will open the Heat Transfer Data Table

Dialog Box (p. ), where you will enter experimental data that defines how heat transfer values relate

to the fluid flow rates (Figure . :The Heat Transfer Data Table Dialog Box (p. )). See Specifying

Heat Exchanger Performance Data (p. ) more details.

Figure . : The Heat Transfer Data Table Dialog Box for the NTU Model

f.

Enter the Auxiliary Fluid Temperature and the Primary Fluid Temperature for the ntu-model.

These are the fixed inlet temperatures at which the test was performed to obtain the heat transfer

data.

g. If the simple-effectiveness-model is chosen, then clicking the Velocity Effectiveness Curve... button,

under the Heat Exchanger Performance Data, allows you to set the velocity and corresponding ef-

fectiveness for each point. More information is available in Specifying Heat Exchanger Performance

Data (p. ).

h. In the Geometry tab, define the heat exchanger macros using the Number of Passes, the Number

of Rows/Pass, and the Number of Columns/Pass fields.The Number of Rows/Pass is along the

auxiliary flow direction (height) and the Number of Columns/Pass is defined in the pass-to-pass

(width) direction. Also, enter the Auxiliary Fluid Inlet Direction and Pass-to-Pass Direction.You

may want to snap the plane tool to either the inlet or outlet of the heat exchanger using the Update

from Plane Tool. Note that the plane tool must be attached exactly and oriented so that its green

arrow points in the auxiliary flow direction, and its blue arrow points in the pass-to-pass direction.

Important

To attach the plane tool exactly, exact coordinates (printed in the console by probing)

of the three corner nodes must be entered in the plane tool (x0, x1, x2) in a specific

order. Also, note that x0 to x1 is the auxiliary flow direction and x1 to x2 is the pass-

to-pass direction.

More information is available in Specifying the Auxiliary Fluid Inlet and Pass-to-Pass Direc-

tions (p. ) and Defining the Macros (p. ).

Figure . : The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Geometry

Tab

Figure . : The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Auxiliary

Fluid Tab

i.

In the Auxiliary Fluid tab, specify the Auxiliary Fluid Properties Method, either as a constant-spe-

cific-heat or as a user-defined-enthalpy.

j.

Auxiliary Fluid Flow Rate, Heat Rejection, Inlet Temperature, and Inlet Pressure can be provided

as a constant, polynomial or piecewise-linear profile that is a function of time. If user-defined-en-

thalpy is selected as the Auxiliary Fluid Properties Method, you will need to specify the Inlet

Quality and the Pressure Drop. More information is available in Specifying the Auxiliary Fluid Prop-

erties and Conditions (p. ).

k.

Click Apply in the Ungrouped Macro Heat Exchanger dialog box to save all the settings. Once you

click the Apply button, the NTU matrix will be computed from the raw data.Therefore, make sure you

click Apply at the very end of your setup.

Important

When you click Apply, look for any error or warning message in the ANSYS Fluent con-

sole. Some of the common errors you may see displayed are due to the NTU compu-

tations not converging. In such cases, check that

you have entered the data correctly

the values of the data are reasonable

the operating condition for the auxiliary fluid flow rate is not too far from the range of

the heat transfer data

Other error messages you may encounter may be due to macros not getting any

cells assigned to it. In such cases, make sure that

the heat exchanger core is rectangular

the directions are correct

you are using uniformly spaced cells in both directions

the mesh is either a hexahedra or wedge and is structured

l.

Repeat steps (a)–(k) for any other heat exchanger fluid zones.

To use multiple fluid zones to define a single heat exchanger, or to connect the auxiliary fluid flow

path among multiple heat exchangers, see Using the Grouped Macro Heat Exchanger Model (p. ).

.... Selecting the Zone for the Heat Exchanger

.... Specifying Heat Exchanger Performance Data

.... Specifying the Auxiliary Fluid Inlet and Pass-to-Pass Directions

.... Defining the Macros

.... Specifying the Auxiliary Fluid Properties and Conditions

.... Setting the Pressure-Drop Parameters and Effectiveness

Choose the fluid zone for which you want to define a heat exchanger in the Fluid Zone drop-down

list.

list.

Based on the heat transfer model you choose in the Model Data tab, some performance data must

be entered for the heat exchanger.

ntu-model: For the ntu-model you will provide the heat transfer for different primary and auxiliary fluid

flow rates. Click the Heat Transfer Data... button to open up a tabular dialog box. Set the number of

auxiliary flow rates and primary fluid flow rates.The dialog box will resize itself accordingly.You will need

to provide various primary fluid flow rates and auxiliary fluid flow rates and the corresponding heat

transfer values.You may write this data to a file that can be read later.

simple-effectiveness-model: For this model, you will need to provide velocity versus effectiveness data.

To provide this you can click the Velocity Effectiveness Curve... button.This will open up a tabular dialog

box. In this dialog box, you can set the number of points in the curve, then you can provide velocities and

corresponding effectiveness values (note that the effectiveness values must be within the range of –).

This data can be written to a file and read back.

To define the auxiliary fluid direction and flow path, you will specify direction vectors for the Auxiliary

Fluid Inlet Direction and the Pass-to-Pass Direction in the Geometry tab. Figure . : 1x4x3

Macros (p. ) shows these directions relative to the macros.

For some problems in which the principal axes of the heat exchanger core are not aligned with the

coordinate axes of the domain, you may not know the auxiliary fluid inlet and pass-to-pass direction

vectors a priori. In such cases, you can use the plane tool as follows to help you to determine these

direction vectors.

. “Snap” the plane tool onto the boundary of the heat exchanger core. (Follow the instructions in Initializing

. Translate and rotate the axes of the tool appropriately until they are aligned with the principal directions

of the heat exchanger core.The depth direction is determined by the red axis, the height direction by

the green axis, and the width direction by the blue axis.

. Once the axes are aligned, click the Update from Plane Tool button in the Ungrouped Macro Heat

Exchanger dialog box.The directional vectors will be set automatically. (Note that the Update from

Plane Tool button will also set the height, width, and depth of the heat exchanger core.)

As discussed in The Macro Heat Exchanger Models (p. ), the fluid zone representing the heat ex-

changer core is split into macros. Macros are constructed based on the specified number of passes,

the number of macro rows per pass, the number of macro columns per pass, and the corresponding

auxiliary fluid inlet and pass-to-pass directions (see Figure . : 1x4x3 Macros (p. )). Macros are

numbered from  to (

) in the direction of auxiliary fluid flow, where  is the number of macros.

Figure . : 1x4x3 Macros

In the Ungrouped Macro Heat Exchanger dialog box, in the Geometry tab, specify the Number of

Passes, the Number of Rows/Pass, and the Number of Columns/Pass. The model will automatically

extrude the macros to the depth of the heat exchanger core. For each pass, the Number of Rows/Pass

are defined in the direction of the auxiliary flow inlet direction and the Number of Columns/Pass

are defined in the direction of the pass-to-pass direction.

Important

The Number of Rows/Pass, as well as the Number of Columns/Pass must be divisible by

the number of cells in their respective directions. For example, if you have  cells in the

auxiliary flow direction, you can use  for the Number of Rows/Pass, but you should not

use  or . If you have  cells in that direction, you can only use  for the Number of

Rows/Pass. The same holds true for the other direction.

.....Viewing the Macros

You can view the auxiliary fluid path by displaying the macros. To view the macros for your specified

Number of Passes, Number of Rows/Pass, and Number of Columns/Pass, click the Apply button

at the bottom of the dialog box, then click the View Passes button to display it. The path of the

auxiliary fluid is color-coded in the display: macro  is red and macro

is blue.

For some problems, especially complex geometries, you may want to include portions of the com-

putational-domain mesh in your macros plot as spatial reference points. For example, you may want

to show the location of an inlet and an outlet along with the macros. This is accomplished by enabling

the Draw Mesh option. The Mesh Display Dialog Box (p. ) will appear automatically when you

enable the Draw Mesh option, where you can set the mesh display parameters. When you click the

View Passes button in the Ungrouped Macro Heat Exchanger dialog box, the mesh display, as

defined in the Mesh Display dialog box, will be included in the macros plot (see Figure . : Mesh

Display With Macros (p. )).

Figure . : Mesh Display With Macros

To define the auxiliary fluid properties and conditions, you will specify the Auxiliary Fluid Flow Rate

(

) in the Auxiliary Fluid tab. The properties of the auxiliary fluid can be specified using the Auxiliary

Fluid Properties Method drop-down list. You can choose a constant-specific-heat (

) and set the

value in the Auxiliary Fluid Specific Heat field below, or as a user-defined function for the enthalpy

using the user-defined-enthalpy option and selecting the corresponding UDF from the Auxiliary

Fluid Enthalpy UDF drop-down list.

The function should return a single value depending on the index:

Enthalpy for given values of temperature, pressure, and quality.

Temperature for given values of enthalpy and pressure

Specific heat for given values of temperature and pressure

The user-defined function should be of type

DEFINE_SOURCE(udf_name, cell_t c, Thread *t, real d[n], int index).

where n in the expression d[n] would be  for temperature,  for pressure, or  for quality. The

variable index is  for enthalpy,  for temperature, or  for specific heat. This user-defined function

should return

real value; /* (temperature or enthalpy or Cp depending on index). */

If you want ANSYS Fluent to compute the auxiliary fluid inlet temperature for a specified heat rejection,

follow the steps below:

. Enable the Fixed Heat Rejection option in the Model Data tab.

. Specify the Heat Rejection (

in Equation . in the Theory Guide) in the Auxiliary Fluid tab.

. Specify the Initial Temperature, which will be used by ANSYS Fluent as an initial guess for the inlet

temperature (

in Equation . and Equation . in the Theory Guide).

If you want ANSYS Fluent to compute the total heat rejection of the core for a given inlet auxiliary fluid

temperature, follow the steps below:

. Enable the Fixed Inlet Temperature option in the Model Data tab.

. Specify the Inlet Temperature (

in Equation . and Equation . in the Theory Guide)

in the Auxiliary Fluid tab.

If you enable the User Defined Enthalpy option under the Auxiliary Fluid Properties Method, you must

also specify the Inlet Pressure (

in Equation . in the Theory Guide) and Inlet Quality (  in Equa-

The pressure drop parameters and effectiveness define the Core Porosity Model. If you would like

ANSYS Fluent to set the porosity of this a heat exchanger zone using a particular core model, you

can select the appropriate model. This will automatically set the porous media inputs. There are three

ways to specify the Core Porosity Model parameters:

Use the values in ANSYS Fluent’s default model.

Define a new core porosity model with your own values.

Read a core porosity model from an external file.

If you do not choose a core porosity model, you will need to set the porosity parameters in the cell

zone conditions dialog box for the heat exchanger zone(s). To do this, follow the procedures described

in User Inputs for Porous Media (p. ).

The models you define will be saved in the case file.

..... Using the Default Core Porosity Model

ANSYS Fluent provides a default model for a typical heat exchanger core. The default-model core

porosity model is a list of constant values from the Ungrouped Macro Heat Exchanger dialog box.

These constants are used for setting the porous media parameters. To use these values, simply retain

the selection of default-model in the Core Porosity Model drop-down list in the Ungrouped Macro

Heat Exchanger dialog box. (You can view the default parameters as described below.)

..... Defining a New Core Porosity Model

If you want to define pressure-drop and effectiveness parameters that are different from those in

the default core porosity model, you can create a new model. The steps for creating a new model

. Click the Edit... button to the right of the Core Porosity Model drop-down list, for which default-

model should have been selected.This will open the Core Porosity Model Dialog Box (p. ) (Fig-

ure . :The Core Porosity Model Dialog Box (p. )).

Figure . : The Core Porosity Model Dialog Box

. Enter the name of your new model in the Name box at the top of the dialog box.

. Under Gas-Side Pressure Drop, specify the following parameters used in Equation . in the Theory

Guide:

Guide:

Minimum Flow to Face Area Ratio ( )

Entrance Loss Coefficient (

)

Exit Loss Coefficient (

)

Gas-Side Surface Area ( )

Minimum Cross Section Flow Area (

)

and the Core Friction Coefficient and Core Friction Exponent (  and , respectively, in Equa-

. Click the Change/Create button.This will add your new model to the database.

..... Reading Heat Exchanger Parameters from an External File

You can read parameters for your Core Porosity Model from an external file. A sample file is shown

below:

("modelname"

(. . . . . . .))

The first entry in the file is the name of the model (for example, modelname). The second set of

numbers contains the gas-side (primary-side) pressure drop parameters:

(

)

To read an external heat exchanger file, you will follow these steps:

. In the Core Porosity Model dialog box, click the Read... button.

. In the resulting Select File dialog box, specify the HXC Parameters File name and click OK. ANSYS

Fluent will read the core porosity model parameters, and add the new model to the database.

.....Viewing the Parameters for an Existing Core Model

To view the parameters associated with a core porosity model that you have already defined, select

the model name in the Database drop-down list (in the Core Porosity Model dialog box). The values

for that model from the database will be displayed in the Core Porosity Model dialog box.

To define a single heat exchanger that uses multiple fluid zones, or to connect the auxiliary fluid flow

path among multiple heat exchangers, you can use heat exchanger groups. To use heat exchanger

groups, perform the following steps:

ON

. Enable the Macro Model Group option and click the Define... button in the Heat Exchanger Model Dialog

Box (p. ) to access the Macro Heat Exchanger Group dialog box.

Edit...

. Specify the inputs to the heat exchanger group in the Macro Heat Exchanger Group dialog box (Fig-

ure . :The Macro Heat Exchanger Group Dialog Box (p. )).

Figure . : The Macro Heat Exchanger Group Dialog Box

a.

Enter the Name of the heat exchanger group.

b. Under Fluid Zones, select the fluid zones that you want to define in the heat exchanger group (Selecting

the Fluid Zones for the Heat Exchanger Group (p. )).

c.

Click the Model Data tab.

i.

Under Primary Fluid Flow Direction, specify the primary fluid flow direction as either Width,

Height, or Depth.

ii.

Under Connectivity, select the Upstream heat exchanger group if such a connection exists (see

Selecting the Upstream Heat Exchanger Group (p. )).

iii. In the Heat Transfer Model drop-down list, choose either the ntu-model or the simple-effective-

ness-model. See step  in Choosing a Heat Exchanger Model (p. ) for details about the differences

between these two models.

iv. From the Core Porosity Model drop-down list, specify the core model that should be used to

calculate the porous media parameters for the zones in the group. More information is available

in Setting the Pressure-Drop Parameters and Effectiveness (p. ).

v.

If the ntu-model is chosen, a Heat Transfer Data... button will appear under Heat Exchanger

Performance Data. Clicking the Heat Transfer Data... button will open the Heat Transfer Data

Table Dialog Box (p. ), where you will enter experimental data that defines how heat transfer

values relate to the fluid flow rates (Figure . :The Heat Transfer Data Table Dialog Box (p. )).

See Specifying Heat Exchanger Performance Data (p. ) more details.

vi. Enter the Auxiliary Fluid Temperature and the Primary Fluid Temperature for the ntu-model.

data.

vii. If the simple-effectiveness-model is chosen, then clicking the Velocity Effectiveness Curve...

button, under the Heat Exchanger Performance Data, allows you to set the velocity and corres-

ponding effectiveness for each point. More information is available in Specifying Heat Exchanger

Performance Data (p. ).

d. Click the Geometry tab (Figure . :The Macro Heat Exchanger Group Dialog Box - Geometry

Tab (p. )).

Figure . : The Macro Heat Exchanger Group Dialog Box - Geometry Tab

i.

Tab (p. )).

i.

Define the heat exchanger macros by specifying the Number of Passes, the Number of Rows/Pass,

and the Number of Columns/Pass. More information is available in Specifying the Auxiliary Fluid

Inlet and Pass-to-Pass Directions (p. ) and Defining the Macros (p. ).

ii.

Specify the Auxiliary Fluid Inlet Direction and Pass-to-Pass Direction (see Specifying the Auxil-

iary Fluid Inlet and Pass-to-Pass Directions (p. )).

e. Click the Auxiliary Fluid tab (Figure . :The Macro Heat Exchanger Group Dialog Box - Auxiliary

Fluid Tab (p. )) to specify the auxiliary fluid operating conditions.

Figure . : The Macro Heat Exchanger Group Dialog Box - Auxiliary Fluid Tab

i.

Specify the Specific Heat as either a constant-specific-heat or as a user-defined-enthalpy.

ii.

Auxiliary Fluid Flow Rate, Initial Temperature, and Inlet Pressure can be provided as a constant,

polynomial or piecewise-linear profile that is a function of time (see Specifying the Auxiliary

Fluid Properties and Conditions (p. )).

f.

If a supplementary auxiliary stream is to be modeled, click the Supplementary Auxiliary Fluid Stream

tab.

Figure . : The Macro Heat Exchanger Group Dialog Box - Supplementary Auxiliary

Fluid Stream Tab

i.

You can specify the Supplementary Mass Flow Rate as a constant, polynomial or piecewise-

linear profile that is a function of time.

ii.

You can specify the Supplementary Flow Temperature as a constant, polynomial or piecewise-

ii.

g. Click Create or Replace in the Macro Heat Exchanger Group dialog box to save all the settings. Re-

place changes the parameters of the already existing group that is selected in the HX Groups list.

Important

Creating or replacing any heat exchanger group initializes any previously calculated

values for temperature and enthalpy for all macros.

. If a heat exchanger group is composed of multiple fluid zones and you want to override any of the inputs

defined in the previous steps, click the Set... button to open the Ungrouped Macro Heat Exchanger

dialog box (Figure . :The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Model Data

Tab (p. )). Select the particular fluid zone as usual. Notice that the individual heat exchanger inherits

the properties of the group by default.You may override any of the following:

Number of Passes, Number of Rows/Pass, and Number of Columns/Pass

Auxiliary Fluid Inlet Direction and the Pass-to-Pass Direction

Core Porosity Model

.... Selecting the Fluid Zones for the Heat Exchanger Group

.... Selecting the Upstream Heat Exchanger Group

.... Specifying the Auxiliary Fluid Properties

.... Specifying Supplementary Auxiliary Fluid Streams

.... Initializing the Auxiliary Fluid Temperature

Select the fluid zones that you want to define in the heat exchanger group in the Fluid Zones drop-

down list. The auxiliary fluid flow in all these zones will be in parallel. Note that one zone cannot be

included in more than one heat exchanger group.

If you want to connect the current group in series with another group, choose the upstream heat

exchanger group. Note that any group can have at most one upstream and one downstream group.

Also, a group cannot be connected to itself. Select a heat exchanger group from the Upstream drop-

down list under Connectivity in the Model Data tab of the Macro Heat Exchanger Group dialog

box.

Important

Connecting to an upstream heat exchanger group can be done only while creating a heat

exchanger group. The connection will persist even if the connection is later changed and

the Replace button is clicked. To change a connection to an upstream heat exchanger

group, you need to delete the connecting group and create a new heat exchanger group

with the proper connection.

The Auxiliary Fluid Inlet Direction and Pass-to-Pass Direction, in the Geometry tab can be specified

as directed in Specifying the Auxiliary Fluid Inlet and Pass-to-Pass Directions (p. ) in the Ungrouped

Macro Heat Exchanger dialog box. Note that the Update from Plane Tool will set the height, width,

and depth as the average of the fluid zones selected in the Fluid Zones.

The auxiliary fluid can be specified as having a constant-specific-heat, or a user-defined function

can be written to calculate the enthalpy, as described in Specifying the Auxiliary Fluid Properties and

The addition or removal of a supplementary auxiliary fluid is allowed in any of the heat exchanger

groups. Note that auxiliary streams are not allowed for individual zones. You will specify the mass

flow rate, temperature, and quality of the supplementary auxiliary fluid. You will also need to specify

the heat transfer for various flow rates of primary and auxiliary flows. The auxiliary stream has the

following assumptions:

The magnitude of a negative auxiliary stream must be less than the primary auxiliary fluid inlet flow rate

of the heat exchanger group.

Added streams will be assumed to have the same fluid properties as the primary inlet auxiliary fluid.

When the heat exchanger group is connected to an upstream heat exchanger group, ANSYS Fluent will

automatically set the initial guess for the auxiliary fluid inlet temperature,

, to be equal to

the

of the upstream heat exchanger group. Thus the boundary condition

for

the first heat exchanger group in a connected series will automatically propagate as an initial guess

for every other heat exchanger group in the series. However, when it is necessary to further improve

convergence properties, you will be allowed to override

for any connected heat exchanger

group by providing a value in the Initial Temperature field. Whenever such an override is supplied,

ANSYS Fluent will automatically propagate the new

to any heat exchanger groups further

downstream in the series. Similarly, every time the

boundary condition for the first heat

exchanger group is modified, ANSYS Fluent will correspondingly update every downstream heat ex-

changer group.

If you want to impose a non-uniform initialization on the auxiliary fluid temperature field, first connect

the heat exchanger groups and then set

for each heat exchanger group in streamwise order.

All heat exchangers included in a group must use the fixed

option. All heat exchangers

within a heat exchanger group must have the same

. In other words, no local override of

this setting is possible through the Ungrouped Macro Heat Exchanger dialog box.

Postprocessing for the heat exchanger models involves computing the total heat rejection rate by setting

up volume monitors and reporting of variables such as computed heat rejection, inlet or outlet temper-

ature, specific heat, and mass flow rate.

Note that when postprocessing dual cell heat exchanger models using dialog boxes other than the

Heat Exchanger Report dialog box (which requires you to explicitly specify whether you want reports

on either the Primary or the Auxiliary fluid), attention must be paid to the fact that there are overlapping

cell zones in the heat exchanger region. For example:

dialog box, you should never select both the primary and the auxiliary fluid zones at the same time. Note

that if no selections are made in this list, then all the cell zones are selected.

that is associated with the primary fluid zone and a surface associated with the auxiliary fluid zone at the

same time, if those surfaces are spatially coincident.

... Heat Exchanger Reporting

...Total Heat Rejection Rate

Reporting the results for the heat exchanger models is done using the Heat Exchanger Report dialog

box.

Results → Reports → Heat Exchanger

Edit...

The following variable options are available for reporting:

Computed Heat Rejection

Inlet Temperature

Outlet Temperature

Specific Heat

.... Computed Heat Rejection

To display the Computed Heat Rejection

. Select Computed Heat Rejection from the Options list.

. Select the Heat Exchanger from the selection list.

. Click Compute.

Figure . : The Heat Exchanger Report Dialog Box for Reporting Computed Heat Rejection

You can write the computed data to a file by clicking the Write... button and entering the name of

the heat exchanger report file in the Select File dialog box.

....Inlet/Outlet Temperature

Inlet/Outlet Temperature can be reported for both primary and auxiliary fluid in the Heat Exchanger

Report dialog box.

Postprocessing for the Heat Exchanger Model

Figure . : The Heat Exchanger Report Dialog Box for Reporting the Inlet Temperature

. Select Inlet Temperature or Outlet Temperature from the Options list.

. Select the heat exchanger from the Heat Exchanger selection list.

. Select either Auxiliary or Primary as the Fluid Zone.

. Select the appropriate boundary zone and report type from the Boundary and Report Type lists, respect-

ively.

Important

Note that the macro heat exchangers (unlike the dual cell heat exchanger) do not

contain an auxiliary cell zone. Hence, the Boundary and Report Type fields will not

appear in the dialog box if you are reporting an auxiliary inlet/outlet temperature.

....Mass Flow Rate

Mass Flow Rate can be reported for both the primary and auxiliary fluid in the Heat Exchanger Report

Figure . : The Heat Exchanger Report Dialog Box for Reporting Mass Flow Rate

. Select Mass Flow Rate from the Options group box.

ively.

Important

Note that the macro heat exchangers (unlike the dual cell heat exchanger) do not contain

an auxiliary cell zone. Hence, the Boundary field will not appear in the dialog box if you

are reporting an auxiliary fluid mass flow rate.

....Specific Heat

Specific Heat for the primary or auxiliary fluid can be reported through the Heat Exchanger Report

dialog box. If specific heat is defined as a function of temperature, the specific heat reported will be

a cell volume averaged value.

Figure . : The Heat Exchanger Report Dialog Box for Reporting Specific Heat

. Select Specific Heat from the Options group box.

To postprocess the total heat rejection rate, you can set up a volume report definition to monitor

convergence and view the computed values.

Solution → Reports → Definitions → New → Volume Report → Sum...

. Select Temperature and Heat Exchanger Source from the Field Variables drop-down lists.

. Select the appropriate Cell Zones and click OK to close the Volume Monitor dialog box.

Figure . : The Volume Report Definition Dialog Box

Important

Note that the macro heat exchangers contain only the primary fluid as the cell zone, but

in case of the dual cell model, you can select either the primary or auxiliary fluid.

To report the results for the macro heat exchangers, you can use the following text command:

define → models → heat-exchanger → macro-model → heat-exchanger-macro-report

Specify the fluid zone

for which you want to obtain information.

To view the connectivity of the heat exchanger groups, use the text command:

(report-connectivity)

Useful Reporting TUI Commands

Chapter : Modeling Species Transport and Finite-Rate Chemistry

Species transport modeling capabilities, both with and without reactions, and the inputs you provide

when using the model are described in this chapter. For theoretical information about species transport,

see Species Transport and Finite-Rate Chemistry in the Theory Guide.

Note that you may also want to consider modeling your turbulent reacting flame using one of the fol-

lowing approaches:

Mixture fraction approach for non-premixed systems (Modeling Non-Premixed Combustion (p. ))

Reaction progress variable approach for premixed systems (Modeling Premixed Combustion (p. ))

Partially premixed approach (Modeling Partially Premixed Combustion (p. ))

Composition PDF Transport approach (Modeling a Composition PDF Transport Problem (p. ))

Multiphase species transport and finite-rate chemistry (Modeling Multiphase Flows (p. ))

For simulations using ANSYS Fluent reacting flow models, you can specify mixtures consisting of up to

chemical species.

The following models and features may not be used with more than  species:

Density-based solver

Eulerian PDF Transport model

Melting/solidification model

Crevice model

Thermal diffusivity model

Surface species

Site species

Note

If the species model is used in combination with a multihpase model, the mass fraction of

a species may be displayed incorrectly in ANSYS CFD-Post if the volume fraction of a cell is

zero. This applies for all ANSYS Fluent files written prior to release  R3.

For all multiphase, multi-species cases created in release . and beyond, the mass fractions

of species will not be available in ANSYS CFD-Post, unless you add the mass fraction of a

species as an additional quantity to be saved in the data file (through the Data File Quant-

ities dialog box).

Information is divided into the following sections:

..Volumetric Reactions

..Wall Surface Reactions and Chemical Vapor Deposition

.. Particle Surface Reactions

.. Electrochemical Reactions

.. Species Transport Without Reactions

.. Reacting Channel Model

.. Reactor Network Model

Information about using species transport and finite-rate chemistry as related to volumetric reactions

is presented in the following subsections. For more information about the theoretical background of

volumetric reactions, see Volumetric Reactions in the Theory Guide.

... Overview of User Inputs for Modeling Species Transport and Reactions

... Enabling Species Transport and Reactions and Choosing the Mixture Material

... Importing a Volumetric Kinetic Mechanism in CHEMKIN Format

... Defining Properties for the Mixture and Its Constituent Species

... Setting up Coal Simulations with the Coal Calculator Dialog Box

... Defining Cell Zone and Boundary Conditions for Species

... Defining Other Sources of Chemical Species

... Solution Procedures for Chemical Mixing and Finite-Rate Chemistry

... Postprocessing for Species Calculations

The basic steps for setting up a problem involving species transport and reactions are listed below.

. Select species transport and volumetric reactions, and specify the mixture material. See Enabling Species

Transport and Reactions and Choosing the Mixture Material (p. ).The mixture material concept is ex-

plained in Mixture Materials (p. ).

. If you are also modeling wall or particle surface reactions, select wall surface and/or particle surface reac-

tions. See Wall Surface Reactions and Chemical Vapor Deposition (p. ) Particle Surface Reactions (p. )

. Check and/or define the properties of the mixture. See Defining Properties for the Mixture and Its Con-

stituent Species (p. ). Mixture properties include the following:

species in the mixture

reactions

other physical properties (for example, viscosity, specific heat)

. Check and/or set the properties of the individual species in the mixture. See Defining Properties for the

Mixture and Its Constituent Species (p. ).

. Set species cell zone and boundary conditions. See Defining Cell Zone and Boundary Conditions for Spe-

cies (p. ).

In many cases, you will not need to modify any physical properties of mixture material because the

solver gets species properties, reactions, and so on, from the materials database when you choose the

mixture material. Some properties, however, may not be defined in the database. You will be warned

when you choose your material if any required properties need to be set, and you can then assign

appropriate values for these properties. You may also want to check the database values of other

Modeling Species Transport and Finite-Rate Chemistry

properties to be sure that they are correct for your particular application. For details about modifying

an existing mixture material or creating a new one from nothing, see Defining Properties for the Mixture

and Its Constituent Species (p. ). Modifications to the mixture material can include the following:

Addition or removal of species

Changing the chemical reactions

Modifying other material properties for the mixture

Modifying material properties for the mixture’s constituent species

If you are solving a reacting flow, you will usually want to define the mixture’s specific heat as a

function of composition, and the specific heat of each species as a function of temperature. You may

want to do the same for other properties as well. By default, most species specific heats in the database

are piecewise-polynomial functions of temperature, but you may choose to specify a different temper-

ature-dependent function if you know of one that is more suitable for your problem.

.... Mixture Materials

The concept of mixture materials has been implemented in ANSYS Fluent to facilitate the setup of

species transport and reacting flow. A mixture material may be thought of as a set of species and a

list of rules governing their interaction. The mixture material carries with it the following information:

A list of the constituent species, referred to as “fluid” materials

A list of mixing laws dictating how mixture properties (density, viscosity, specific heat, and so on) are to

be derived from the properties of individual species if composition-dependent properties are desired

A direct specification of mixture properties if composition-independent properties are desired

Diffusion coefficients for individual species in the mixture

Other material properties (for example, absorption and scattering coefficients) that are not associated

with individual species

A set of reactions, including a reaction type (finite-rate, eddy-dissipation, and so on) and stoichiometry

and rate constants

The mixture materials are stored in the ANSYS Fluent materials database. Many common mixture

materials are included (for example, methane-air, propane-air). Generally, one or two-step reaction

mechanisms and many physical properties of the mixture and its constituent species are defined in

the database.

The ANSYS Fluent materials database is accessed in one of two ways, depending on the sequence of

your workflow:

through the Species Model dialog box before any one of the species models is enabled

through the Create/Edit Materials dialog box after one of the available species models is enabled

When you enable one of the species models, the mixture material that you have selected for your

application, its constituent fluid materials, and properties will be loaded into your simulation. If any

necessary information about the selected material (or the constituent fluid materials) is missing, the

solver will inform you that you need to specify it. In addition, you may choose to modify any of the

Volumetric Reactions

predefined properties. See Using the Create/Edit Materials Dialog Box (p. ) for information about

the sources of ANSYS Fluent database property data.

For example, if you plan to model combustion of a methane-air mixture using global kinetics, you

do not need to explicitly specify the species involved in the reaction or the reaction itself. You will

simply select methane-air as the mixture material to be used, and the relevant species (CH4, O2, CO2,

H2O, and N2) and reaction data will be loaded into the solver from the database. You can then check

the species, reactions, and other properties and define any properties that are missing and/or modify

any properties for which you want to use different values or functions. You will generally want to

define a composition- and temperature-dependent specific heat, and you may want to define addi-

tional properties as functions of temperature and/or composition.

The use of mixture materials gives you the flexibility to select and load from the Fluent database one

of the many predefined mixtures that is appropriate for your case or, if you want to create your own

custom mixture material, a mixture-template (the default) consisting of H2O, O2, and N2. Once the

mixture material has been copied to the solver, you can modify it in the Create/Edit Materials Dialog

Box (p. ), as described in Defining Properties for the Mixture and Its Constituent Species (p. ).

... Enabling Species Transport and Reactions and Choosing the Mixture

Material

Material

The problem setup for species transport and volumetric reactions begins in the Species Model dialog

box (Figure . : The Species Model Dialog Box (p. )). For cases that involve multiphase species

transport and reactions, refer to Modeling Species Transport in Multiphase Flows in the Theory Guide.

Edit...

Figure . : The Species Model Dialog Box

. Under Model, select Species Transport.

. Under Reactions, select Volumetric.

. In the Mixture Material drop-down list under Mixture Properties, select which mixture material you

want to use in your problem or, if you want to create your own mixture material, retain the default selection

of mixture-template consisting of H2O, O2, and N2.The drop-down list  includes all of the mixtures that

are currently defined in the database. If there is a mixture material listed that is similar to your desired

mixture, you may choose that material and modify it following the steps provided in Defining Properties

for the Mixture and Its Constituent Species (p. ).

The number of species in the selected mixture material is displayed in the Number of Volumetric

Species field and, if applicable, in the Number of Solid Species and Number of Site Species

fields. To review the mixture composition and reactions of the selected Fluent database mixture

material, click the View... button to the right of Mixture Material. This opens the Fluent Database

Materials dialog box. Clicking, in turn, the View... buttons next to Mixture Species and Reaction

opens the corresponding dialog boxes allowing you to examine the constituent species and reactions

data. Note, that the mixture properties cannot be edited before the mixture material is copied to

your Fluent problem. For this reason, all related controls are dimmed while viewing the mixture

When you enable the species transport model by clicking either OK or Apply, ANSYS Fluent performs

The selected Fluent database mixture material including all constituent fluid materials (species)

and properties are automatically copied to your case and appear under Mixture in the tree and

the Materials task page.

If any properties for the selected mixture material (or the constituent fluid materials) are missing,

the solver prints to the console a notice of the required data.

When the mixture material is copied, the Mixture Material drop-down list in the Species Model

dialog box changes to contain only the mixtures defined for your Fluent problem.

The View... button is replaced by the Edit... button giving you an option to access the Edit

Material dialog box (Edit Material Dialog Box (p. )) from the Species Model dialog box.

The Create/Edit Materials dialog box lists mixture in the Material Type drop-down list allowing

you to access the Fluent mixture material database. If you want to check or modify any properties

of the mixture material, use the Create/Edit Materials Dialog Box (p. ), as described in Defining

Properties for the Mixture and Its Constituent Species (p. ).

You can add more mixture materials to your case by copying them from the database, as described

in Copying Materials from the ANSYS Fluent Database (p. ), or by creating a new mixture, as

described in Creating a New Material (p. ) and Defining Properties for the Mixture and Its Con-

stituent Species (p. ).

. Select the Turbulence-Chemistry Interaction (TCI) modeling option.The following options are available:

Finite-Rate/No TCI

computes only the Arrhenius rate (see Equation . in the Theory Guide) and neglects turbulence-

chemistry interaction.This model is recommended for laminar or turbulent flows using complex

chemistry where either the turbulence time-scales are expected to be fast relative to the chemistry

time scales or where the chemistry is sufficiently complex that the chemistry timescales of importance

are highly disparate throughout the simulation.You can specify the following inputs:

Flow Iterations per Chemistry Update (steady-state only)

Increasing the number reduces the computational expense of the chemistry calculations. By default,

ANSYS Fluent will update the chemistry once per flow iteration.This option is not available when

the None - Explicit Source  option is selected for Chemistry Solver.

Aggressiveness Factor (steady-state only)

This is a numerical factor that controls the robustness and the convergence speed.This value

ranges between  and , where  is the most robust, but results in the slowest convergence.The

default value for the Aggressiveness Factor is ..This option is available only when Stiff

Chemistry Solver or CHEMKIN CFD Solver is selected for Chemistry Solver.

Temperature Threshold (steady-state only)

The reaction rate is highly temperature-dependent.When temperature is low, the reaction rate

is fairly small and can be ignored.This may reduce the computational cost without sacrificing ac-

curacy. ANSYS Fluent sets the chemistry reaction rate to zero in cells where temperature is below

the Temperature Threshold you specified.The default value is  K.This option is available

only when Stiff Chemistry Solver or CHEMKIN CFD Solver is selected for Chemistry Solver.

Finite-Rate/Eddy-Dissipation (turbulent flows only)

computes both the Arrhenius rate and the mixing rate and uses the smaller of the two.

Eddy-Dissipation (turbulent flows only)

computes only the mixing rate (see Equation . and Equation . in the Theory Guide).

Eddy-Dissipation Concept (turbulent flows only)

models turbulence-chemistry interaction with detailed chemical mechanisms (see Equation . and

Equation . in the Theory Guide).When using this model, you can modify the following:

ANSYS Fluent will update the chemistry once per flow iteration.

default value for the Aggressiveness Factor is ..

the Temperature Threshold you specified.The default value is  K.

Volume Fraction Constant , Time Scale Constant

in Equation . in the Theory Guide.The default values are recommen-

ded.

. From the Chemistry Solver drop-down list, select the solver for your simulation (note that the solvers

available in the drop-down list are dependant on the selected Turbulence-Chemistry Interaction model):

If you want the stiff chemistry to relax to chemical equilibrium without solving reactions, select Relax

to Chemical Equilibrium.This option is not available for Eddy Dissipation Concept. For information

about the Relaxation to Chemical Equilibrium model, refer to The Relaxation to Chemical Equilibrium

Model in the Theory Guide

Important

The Relax to Chemical Equilibrium chemistry solver requires thermodynamic data

of all species to calculate chemical equilibrium. You can supply your own database

using the Import CHEMKIN Format Mechanism dialog box (opened by clicking Import

CHEMKIN mechanism...) (see Importing a Volumetric Kinetic Mechanism in CHEMKIN

Format (p. ) and Importing a Surface Kinetic Mechanism in CHEMKIN Format (p. )

for details). A sample database is also contained in the file .../flu-

entx.x/cpropep/data/thermo.db. If you define your own species in ANSYS

Fluent, as determined by the Chemical Formula in the Create/Edit Materials dialog

box, and this species name is not in the thermo.db file, ANSYS Fluent will report an

error. To overcome this error, you must manually enter all the unknown species in

the thermo file.

If you want to solve finite-rate chemistry, select either Stiff Chemistry Solver or CHEMKIN-CFD Solver.

These two solvers are available when using the Finite-Rate/No TCI or Eddy-Dissipation Concept TCI

option.

Selecting CHEMKIN-CFD Solver will enable you to use the ANSYS CHEMKIN-CFD solution al-

gorithms, which are based on and compatible with the ANSYS Chemkin-Pro technology. Once

you click OK or Apply, you will be prompted to import a CHEMKIN mechanism, if you have not

already done so. Refer to the ANSYS Chemkin-Pro Input and Theory manuals for details on the

chemistry formulation options. See Using ANSYS Encrypted Mechanisms (p. ) for instructions

on establishing a CHEMKIN-mechanism based material. In addition, Appendix C: Controlling

CHEMKIN-CFD Solver Parameters Using Text Commands (p. ) includes information about ad-

vanced solver settings and diagnostic information for the CHEMKIN-CFD solver. With the Chemkin-

CFD Solver selected, the methods for mixture material properties will be defaulted to chemkin.

See Procedure for Importing Volumetric CHEMKIN Mechanisms (p. ) for details.

If you want to make explicit use of chemistry source terms in the species transport equations, without

a stiff-chemistry solver, select None - Explicit Source.This solver is not recommended for stiff or

complex chemistry.

. (optional) For TCI model options that consider finite-rate chemistry, set the integration parameters using

the Integration Parameters dialog box (opened by clicking the Integration Parameters... button). In

the Integration Parameters dialog box, you can select acceleration methods (see Using Chemistry Accel-

eration (p. ) for more details):

Dynamic Mechanism Reduction (DMR) (for Stiff Chemistry Solver): See Using Dynamic Mechanism

Reduction (p. ) for details.

Chemistry Agglomeration (CA) (for Stiff Chemistry Solver and Relax to Chemical Equilibrium): See

Using Chemistry Agglomeration (p. ) for details.

ISAT: See Using ISAT (p. ) for details.

Dynamic Cell Clustering (DCC) (for the CHEMKIN-CFD Solver): See see Using Dynamic Cell Cluster-

ing (p. ) for details.

. (optional) Select any Options desired. If you want to model full multicomponent (Stefan-Maxwell) diffusion

or thermal (Soret) diffusion, select the Full Multicomponent Diffusion or Thermal Diffusion option,

See Full Multicomponent Diffusion (p. ) for details.

. Enable the Thickened Flame Model when modeling unsteady laminar flames, or when using an LES

model for turbulent premixed and partially-premixed flames. In the Thickened Flame Model Options

group box, specify:

Number of Grid Points in Flame: Default is  grid points.

(simulations with LES only) Integral Length Scale: Is the representative of the largest eddy sizes,

in

in

Equation . in the Fluent Theory Guide.You should provide a value based on the geometry and size

of the characteristic bodies (such as inlet, burners, or bluff bodies).Typically, a value ranging from /

to / of the characteristic dimension is used.

Consequently, in the Create/Edit Materials dialog box, you will specify the Laminar Flame Speed,

for which you have a choice of constant, user-defined, or metghalchi-keck-law, and the Laminar

Flame Thickness, for which you have a choice of constant, user-defined, or diffusivity-over-

flame-speed.

Note

Since the thickened flame model must capture the correct flame speed, it is imper-

ative that the combination of your chemical mechanism and your molecular transport

properties (diffusion coefficients and thermal conductivity) reproduce the correct

laminar flame speed. It is recommended that you verify this with a 1D premixed

flame simulation using ANSYS Chemkin-Pro, for example.

When the Thickened Flame Model is enabled (Figure . : The Species Model Dialog Box Displaying

the Thickened Flame Model (p. )), you have the option to hook a UDF in the User-Defined

Function Hooks dialog box to customize the Thickened Flame Model parameters. Refer to

DEFINE_THICKENED_FLAME_MODEL in the Fluent Customization Manual for details.

Important

The Thickened Flame Model is available only for unsteady laminar or turbulent

(LES / DES / SAS / SBES / SDES) flows, with Species Transport and Volumetric

Reactions enabled.

For information about the theory behind the Thickened Flame Model, refer to The Thickened

Flame Model in the Theory Guide.

Figure . : The Species Model Dialog Box Displaying the Thickened Flame Model

The Species Model Dialog Box

. (optional) Select the species for which you want to specify boundary conditions. Only the species that

you have selected will be listed in the relevant boundary condition dialog boxes.This will facilitate the

problem setup, especially when a large number of species are used in a gas mixture. Note that the Patch

and Hybrid Initialization dialog boxes, as well as the Solution Initialization task page will also display

only the selected species.

a.

Click Select Boundary Species.

Figure . : The Select Boundary Species Dialog Box

By default, all the gas species for which the transport equations are to be applied are set as

boundary species and appear in the Selected multiple-selection list of the Select Boundary

Species dialog box (see Figure . : The Select Boundary Species Dialog Box (p. )).

b. Modify the boundary species list as follows:

To remove the species from the Selected Species multiple-selection list, select it and click Remove.

The species will be moved from the Selected Species list to the Unselected Species list.

To add the species back to the Selected Species list, simply select it in the Unselected Species

multiple-selection list and click Add.The species will be moved from the Unselected Species list

to the Selected Species list.

. (optional) In a similar manner, click the Select Reported Residuals button and select the species that

you want to monitor. Only the residuals for the selected species will be monitored and plotted in the

graphics window during the simulation.

Figure . : The Select Residual Monitored Species

By default, all the species for which the species transport equations are to be solved are set as

monitored species, and their residual plots will be drawn in the graphics window during the run.

For a large number of monitored species, it may be difficult to distinguish the overlapping plot

lines. By decreasing the number of monitored species, you can obtain clearer residual plots.

Important

The Fluent solver performs the convergence checks only for the monitored species.To prevent

false convergence, make sure to include the species that may have difficulties converging

in the monitored species list.

You can modify the list of the monitored species dynamically during a run.

You can import gas kinetics mechanism in CHEMKIN format, which can be used with any solver option.

For the CHEMKIN-CFD Solver, native CHEMKIN computations will determine reaction rates, so full

compatibility with ANSYS Chemkin-Pro is provided.

Note

If a mechanism includes at least one reaction type that is not supported in the Fluent ma-

terial-definition interface (that is, it is not included in the options for manual setup of reac-

tions), the reactions of the CHEMKIN mechanism will not be displayed in the Fluent interface,

even though they will be correctly used in Fluent computations.

.... Using ANSYS Encrypted Mechanisms

For certain types of simulations, Fluent supports the use of encrypted gas kinetics mechanisms, such

as those derived from the ANSYS Model Fuels Library (encrypted) or through ANSYS services. In order

to use an encrypted mechanism, you must first import both the gas-phase kinetics and thermodynamic

files as described in Procedure for Importing Volumetric CHEMKIN Mechanisms (p. ).

When using encrypted CHEMKIN gas mechanisms, note the following points:

Encrypted mechanisms can only be used with the CHEMKIN-CFD solver or the Relax to Chemical Equilib-

rium option

Prior to importing a flamelet or reading a PDF table generated with an encrypted mechanism, you must

first import the mechanism

Chemical equilibrium PDF table generation is not supported

Multiphase and Decoupled Detailed Chemistry models are not supported

You cannot combine encrypted and plain-text gas kinetics, surface kinetics and thermodynamics files in

a simulation

The chemistry acceleration options Dynamic Mechanism Reduction (DMR) and Dimension Reduction (DR)

are not supported.

Note

The proprietary reaction data will not be displayed in the Fluent interface.

.... Procedure for Importing Volumetric CHEMKIN Mechanisms

You can import the CHEMKIN mechanism file into ANSYS Fluent using the Import CHEMKIN Format

Mechanism dialog box (Figure . : The Import CHEMKIN Format Mechanism Dialog Box for Volumetric

Kinetics (p. )) (opened by clicking Import CHEMKIN Mechanism... in the Species Model dialog

box).

Figure . : The Import CHEMKIN Format Mechanism Dialog Box for Volumetric Kinetics

box).

In the Import CHEMKIN Format Mechanism dialog box

. Enter a name for the chemical mechanism under Material Name.

. Enter the path to the CHEMKIN file (for example, path/file.inp) in the Kinetics Input File text

field in the Gas-Phase group box.

Important

Since ANSYS Fluent does not solve for the last species, you must ensure that the last

species in the CHEMKIN mechanism species list is an abundant species, such as nitrogen.

If not, edit the CHEMKIN mechanism file before importing it into ANSYS Fluent, and

move the most abundant species (that is the species in your system with the largest

total mass fraction) to the end of the species list.

. Specify species thermodynamic property data.You can include the data in the kinetics input file and/or

in a separate file as follows:

If you want to specify thermodynamic data for all species in the kinetics input file, enable All contained

in Kinetics Input File to avoid the need to specify a separate file.

If you provide some or all species thermodynamic data in a separate file, disable All contained in

Kinetics Input File and specify the thermodynamic data file location.

You can either use the default thermodynamic database file, thermo.db, provided in the

cpropep\data directory in your ANSYS Fluent installation area or specify the path of your

thermodynamic database file if thermo.db does not contain all the gas-phase species in the

CHEMKIN mechanism. The format for thermo.db is detailed in the CHEMKIN manual  [] (p. ).

. (optional) To import transport property data, enable Import database under Transport Property Data

(Optional) and specify the location of the species transport property data.You can include the data in

the kinetics input file and/or in a separate file as follows:

If you want to specify transport property data for all species in the kinetics input file, enable All con-

tained in Kinetics Input File, to avoid the need to specify a separate file.

If you want to provide some or all species transport data in a separate file, disable All contained in

Kinetics Input File and specify the transport property data file location.

ANSYS Fluent will enable mixture-averaged multicomponent diffusion and set the Lennard-Jones

kinetic theory parameters for all the species in the imported CHEMKIN mechanism. If you would

like to use Stefan-Maxwell diffusion, enable the Full Multicomponent Diffusion in the Species

Once the CHEMKIN files are imported, ANSYS Fluent creates a material with the specified name,

which will contain the data for the species and reactions, and add it to the list of available Mixture

Materials in the Create/Edit Materials Dialog Box (p. ). The methods to compute the mixture's

material properties are set automatically depending on which chemistry solver you selected.

For cases with imported transport property data, the methods used to calculate properties are

shown in the table below.

CHEMKIN-CFD Solver

Stiff Chemistry Solver

Material Property

chemkin [ a ]

mixing law

ideal-gas-mixing-law

Viscosity

kinetics-theory

Mass Diffusivity

mixing law

Viscosity

Thermal Diffusion

a.

The material property value will be computed by ANSYS Chemkin-Pro. You may choose

to use a different property method if it is more suitable for your problem.

For cases with the CHEMKIN-CFD Solver that do not use transport property data, only the Spe-

cific Heat mixture property will be automatically set to the chemkin method.

Note that when Full Multicomponent Diffusion is enabled in the Species dialog box, ANSYS

Chemkin-Pro returns full multicomponent diffusivities. If Full Multicomponent Diffusion is disabled,

ANSYS Chemkin-Pro returns mixture averaged mass diffusivities for each species.

Figure . : The Material Dialog Box When Importing CHEMKIN Transport Properties

. Click the Import button.

Once you click Import, ANSYS Fluent automatically saves the reaction mechanism and thermal

files in the data structure. The original input files are not required to be retained along with the

Fluent case file. ANSYS Fluent will automatically regenerate these files as needed (for example,

when using the CHEMKIN-CFD solver).

For information on how to import a surface kinetic mechanism in CHEMKIN format, see Importing a

Surface Kinetic Mechanism in CHEMKIN Format (p. ).

.... CHEMKIN Mechanisms Included with ANSYS Fluent

A CHEMKIN mechanism is a chemical reaction mechanism (also called a chemistry set) that has the

following mechanism components:

A file containing thermochemical data for the chemical species of interest

A file containing a description of the reactions occurring in the gas phase

(Optional) A file containing a description of the reactions occurring at the gas-surface interface or on the

surface

(Optional) A file containing gas-phase transport data

A set of gas-phase and/or surface reactions are generally developed using specific thermochemical

data. Thus, the gas-phase kinetics, surface kinetics, and thermodynamic data are treated as a chemistry

“set” in reacting-flow simulations. ANSYS Fluent provides the following fuel-combustion mechanisms

(including reactions, thermodynamic data, and transport data) that are appropriate for use in common

combustion simulations:

Methane / Ethane: -species version of GRI-Mech . (grimech30_50spec)

This is the original GRI-mech . ( species) [] (p. ) with three species (argon AR, propane

C3H8, and propyl radical C3H7) and their reactions removed.

In fuel/air or fuel/oxygen combustion, the removal of these species is expected to have negligible

effect on the mechanism predictive capabilities for methane and ethane as fuels. The applicability

of the GRI mechanism and validation cases are provided on the GRI mechanism web site [] (p. ).

Propane: -species high-temperature mechanism (Propane-NOx_highT)

The mechanism has  elementary reaction steps and was obtained by removing species and re-

actions that are unimportant for propane combustion from the comprehensive master mechanism

[] (p. ). ANSYS Chemkin-Pro Reaction Workbench software was used to reduce the master

mechanism under the conditions of slightly lean and high pressure laminar flame of a propane/air

mixture using the Directed Relation Graph (DRG) method.

Two hydrogen mechanisms:

– -species version for H2 combustion (H2_mech)

The mechanism has  elementary reaction steps and has been extracted from the Li et al.

[] (p. ) mechanism for CO and other hydrocarbons.

– -species version for H2 combustion with NOx (H2_NOx_mech)

The mechanism has  elementary reaction steps. The hydrogen combustion sub-mechanism

is the same as the H2_mech mechanism, above. The NOx sub-mechanism is based on the study

by the Glarborg group [] (p. ).

As discussed in Overview of User Inputs for Modeling Species Transport and Reactions (p. ), if you

use a mixture material from the ANSYS Fluent database, most mixture and species properties will

already be defined. You may follow the procedures in this section to check the current properties,

modify some of the properties, or set all properties for a brand-new mixture material that you are de-

fining from nothing.

Remember that you will need to define properties for the mixture material and also for its constituent

species. It is important that you define the mixture properties before setting any properties for the

constituent species, since the species property inputs may depend on the methods you use to define

the properties of the mixture.

The recommended sequence for property inputs is as follows:

. Define the mixture species, and reaction(s), and define physical properties for the mixture. Remember to

click the Change/Create button when you are done setting properties for the mixture material.

. Define physical properties for the species in the mixture. Remember to click the Change/Create button

after defining the properties for each species.

These steps, all of which are performed in the Create/Edit Materials Dialog Box (p. ), are described

in detail in this section.

Setup →

Materials

.... Defining the Species in the Mixture

In the Create/Edit Materials dialog box (Figure . : The Create/Edit Materials Dialog Box (Showing

a Mixture Material) (p. )), check that the Material Type is set to mixture and your mixture is selected

in the Fluent Mixture Materials list.

Figure . : The Create/Edit Materials Dialog Box (Showing a Mixture Material)

Click the Edit... button to the right of Mixture Species under the Properties group box and in the

Species Dialog Box (p. ) (Figure . : The Species Dialog Box (p. )) that opens define the species

in the mixture material.

Figure . : The Species Dialog Box

Important

For Chemkin mechanisms, the recommended approach for modifying mixture materials is

to modify the Chemkin mechanism file and then re-import it into your Fluent case.

..... Overview of the Species Dialog Box

In the Species dialog box, the Selected Species list shows all of the fluid-phase species in the mixture.

If you are modeling wall or particle surface reactions, the Selected Solid Species list will show all

of the bulk solid species in the mixture. Solid species are species that are deposit to, or etch from,

wall boundaries or discrete-phase particles (for example, Si(s)) and do not exist as fluid-phase species.

If you are modeling wall surface reactions with site balancing, where species adsorb onto the wall

surface, react, and then desorb off the surface, the Selected Site Species list will show all of the

site species in the mixture.

The use of solid and site species with wall surface reactions is described in Wall Surface Reactions

and Chemical Vapor Deposition (p. ). See Particle Surface Reactions (p. ) for information about

particle surface reactions.

Important

The order of the species in the Selected Species list is very important. ANSYS Fluent con-

siders the last species in the list to be the bulk species. You should therefore be careful

to retain the most abundant species (by mass) as the last species when you add species

to or delete species from a mixture material.

The Available Materials list shows materials that are available but not in the mixture. Generally,

you will see air in this list, since air is always available by default.

..... Adding Species to the Mixture

If you are creating a mixture from nothing or starting from an existing mixture and adding some

missing species, you will first need to load the desired species from the database (or create them,

if they are not present in the database) so that they will be available to the solver. You will need to

close the Species dialog box before you begin, since it is a “modal” dialog box that will not allow

you to do anything else when it is open. The procedure for adding species is as follows:

. In the Create/Edit Materials dialog box, click the Fluent Database... button to open the Fluent

Database Materials dialog box and copy the desired species, as described in Copying Materials from

the ANSYS Fluent Database (p. ). Remember that the constituent species of the mixture are fluid

materials, so you should select fluid as the Material Type in the Fluent Database Materials dialog

box to see the correct list of choices. Note that available solid and site species (for surface reactions)

are also contained in the fluid list.

Important

If you do not see the species you are looking for in the database, you can create a

new fluid material for that species, following the instructions in Creating a New Mater-

ial (p. ), and then continue with step , below.

. Re-open the Species dialog box.You will see that the fluid materials you copied from the database (or

created) are listed in the Available Materials list.

. To add a species to the mixture, select it in the Available Materials list and click the Add button below

the Selected Species list (or below the Selected Site Species or Selected Solid Species list, to define

a site or solid species).The species will be added to the end of the relevant list and removed from the

Available Materials list.

. Repeat the previous step for all the desired species.When you are finished, click the OK button.

Important

Adding a species to the list will alter the order of the species. You should be sure that

the last species in the list is the bulk species, and you should check all cell and boundary

Important

zone conditions, under-relaxation factors, and other solution parameters that you have

set, as described in detail in the following sections.

..... Removing Species from the Mixture

To remove a species from the mixture, simply select it in the Selected Species list (or the Selected

Site Species or Selected Solid Species list) and click the Remove button below the list. The species

will be removed from the list and added to the Available Materials list.

Important

Removing a species from the list will alter the order of the species.You should be sure that

the last species in the list is the bulk species, and you should check any cell zone or boundary

conditions, under-relaxation factors, or other solution parameters that you have set, as de-

scribed in detail in the following sections.

Any species that is a reactant, product, or enhanced third-body in an active reaction cannot

be deleted from the mixture material.

..... Assigning the Last Species

If you find that the last species in the Selected Species list is not the most abundant species (as it

should be), you will need to rearrange the species to obtain the proper order.

. Select the bulk species in the Selected Species list.

. Click Last Species.The selected species will be placed at the end of the Selected Species list.The

transport equation of the last species will not be solved.

.....The Naming and Ordering of Species

As discussed previously, you should retain the most abundant species as the last one in the Selected

Species list when you add or remove species. Additional considerations you should be aware of

when adding and deleting species are presented here.

There are three characteristics of a species that identify it to the solver: name, chemical formula, and

position in the list of species in the Species dialog box. Changing these characteristics will have the

following effects:

You can change the Name of a species (using the Create/Edit Materials Dialog Box (p. ), as described

in Renaming an Existing Material (p. )) without any consequences.

You should never change the given Chemical Formula of a species.

You will change the order of the species list if you add or remove any species.When this occurs, all cell

zone or boundary conditions, solver parameters, and solution data for species will be reset to the default

values. (Solution data, cell zone or boundary conditions, and solver parameters for other flow variables

will not be affected.) Therefore, if you add or remove species you should take care to redefine species

cell zone and boundary conditions and solution parameters for the newly defined problem. In addition,

you should recognize that patched species concentrations or concentrations stored in any data file that

was based on the original species ordering will be incompatible with the newly defined problem.You

can use the data file as a starting guess, but you should be aware that the species concentrations in the

data file may provide a poor initial guess for the newly defined model.

.... Defining Reactions

If your ANSYS Fluent model involves chemical reactions, you can define the reactions in which the

defined species participate. This will be necessary only if you are creating a mixture material from

nothing, you have modified the species, or you want to redefine the reactions for some other reason.

Depending on which turbulence-chemistry interaction model you selected in the Species Model

dialog box (see Enabling Species Transport and Reactions and Choosing the Mixture Material (p. )),

the appropriate reaction model will be displayed in the Reaction drop-down list in the Edit Material

dialog box. If you are using the Finite-Rate/No TCI or Eddy-Dissipation Concept model, the reaction

model will be finite-rate; if you are using the Eddy-Dissipation model, the reaction model will be

eddy-dissipation; if you are using the Finite-Rate/Eddy-Dissipation model, the reaction model will

be finite-rate/eddy-dissipation.

..... Inputs for Reaction Definition

To define the reactions, click the Edit... button to the right of Reaction. The Reactions dialog box

(Figure . : The Reactions Dialog Box (p. )) will open.

Figure . : The Reactions Dialog Box

The steps for defining reactions are as follows:

. Set the total number of reactions (volumetric reactions, wall surface reactions, and particle surface re-

actions) in the Total Number of Reactions field. Use the arrows to change the value, or type in the

value and press Enter.

Note that if your model includes discrete-phase combusting particles, you should include the

particulate surface reaction(s) (for example, char burnout, multiple char oxidation) in the number

of reactions only if you plan to use the multiple surface reactions model for surface combustion.

. Specify the Reaction Name of the reaction you want to define.

. Set the ID of the reaction you want to define. Again, if you type in the value be sure to press Enter.

. If this is a fluid-phase reaction, keep the default selection of Volumetric as the Reaction Type. If this

is a wall surface reaction (described in Wall Surface Reactions and Chemical Vapor Deposition (p. ))

or a particle surface reaction (described in Particle Surface Reactions (p. )), select Wall Surface or

Particle Surface as the Reaction Type. See User Inputs for Particle Surface Reactions (p. ) for further

information about defining particle surface reactions.

. Specify how many reactants and products are involved in the reaction by increasing the value of the

Number of Reactants and the Number of Products. Select each reactant or product in the Species

drop-down list and then set its stoichiometric coefficient and rate exponent in the appropriate Stoi-

ch. Coefficient and Rate Exponent fields.The stoichiometric coefficient is the constant

or

in

Equation . in the Theory Guide and the rate exponent is the exponent on the reactant or product

concentration,

or

in Equation . in the Theory Guide.

There are two general classes of reactions that can be handled by the Reactions dialog box, so

it is important that the parameters for each reaction are entered correctly. The classes of reactions

Global forward reaction (no reverse reaction): Product species generally do not affect the forward

rate, so the rate exponent for all products (

) should be . For reactant species, set the rate exponent

(

) to the desired value. If such a reaction is not an elementary reaction, the rate exponent will

generally not be equal to the stoichiometric coefficient (

) for that species. An example of a global

forward reaction is the combustion of methane:

(.)

where

,

,

,

,

,

,

, and

.

Figure . : The Reactions Dialog Box (p. ) shows the coefficient inputs for the combustion

of methane. See also the methane-air mixture material in the Fluent Database Materials Dialog

Box (p. ).

Note that, in certain cases, you may want to model a reaction where product species affect

the forward rate. For such cases, set the product rate exponent (

) to the desired value. An

example of such a reaction is the gas-shift reaction (see the carbon-monoxide-air mixture

material in the Fluent Database Materials Dialog Box (p. )), in which the presence of water

has an effect on the reaction rate:

In the gas-shift reaction, the rate expression may be defined as:

(.)

where

,

,

,

,

,

,

, and

.

Reversible reaction: An elementary chemical reaction that assumes the rate exponent for each species

is equivalent to the stoichiometric coefficient for that species. An example of an elementary reaction

is the oxidation of SO2 to SO3:

where

,

,

,

,

, and

.

See step  below for information about how to enable reversible reactions.

where

,

,

,

,

, and

.

. If you are using the laminar finite-rate, finite-rate/eddy-dissipation, eddy-dissipation concept or PDF

transport model for the turbulence-chemistry interaction, enter the following parameters for the

Arrhenius rate in the Arrhenius Rate group box:

Note

All quantities for the Arrhenius rate parameters are in units of kgmol, m3, and seconds.

Pre-Exponential Factor

(the constant

in Equation . in the Theory Guide).The units of

must be specified such that

the units of the molar reaction rate,

in Equation . in the Theory Guide, are moles/volume-time

(for example, kmol/

s) and the units of the volumetric reaction rate,

in Equation . in the

Theory Guide, are mass/volume-time (for example, kg/

s).

Important

It is important to note that if you have selected the British units system, the

Arrhenius factor should still be entered in SI units. This is because ANSYS Fluent

applies no conversion factor to your input of

(the conversion factor is .) when

you work in British units, as the correct conversion factor depends on your inputs

for

,

, and so on.

Activation Energy

in the forward rate constant expression, Equation . in the Theory Guide).

Temperature Exponent

(the value for the constant

Third-Body Efficiencies

(the values for

in Equation . in the Theory Guide). If you have accurate data for the efficiencies

and want to include this effect on the reaction rate (that is, include  in Equation . in the Theory

Guide), select the Third Body Efficiencies option and click the Specify... button to open the Third-

Body Efficiency Dialog Box (p. ) (Figure . :The Third-Body Efficiency Dialog Box (p. )).

For each Species in the dialog box, specify the Third-Body Efficiency.

Important

It is not necessary to include the third-body efficiencies. You should not enable

the Third-Body Efficiencies option unless you have accurate data for these

Figure . : The Third-Body Efficiency Dialog Box

Pressure-Dependent Reaction

(if relevant) If you are using the laminar finite-rate or eddy-dissipation concept model for turbulence-

chemistry interaction, or have selected the composition PDF transport model (see Modeling a

Composition PDF Transport Problem (p. )), and the reaction is a pressure fall-off reaction (see

Pressure-Dependent Reactions in the Theory Guide), enable the Pressure-Dependent Reaction

option for the Arrhenius Rate and click the Specify... button to open the Pressure-Dependent

Reaction dialog box (Figure . :The Pressure-Dependent Reaction Dialog Box (p. )).

Figure . : The Pressure-Dependent Reaction Dialog Box

Under Reaction Parameters, select the appropriate Reaction Type (lindemann, troe, or

sri). See Pressure-Dependent Reactions in the Theory Guide for details about the three

methods. Next, specify if the Bath Gas Concentration (

Guide) is to be defined as the concentration of the mixture, or as the concentration of one

of the mixture’s constituent species, by selecting the appropriate item in the drop-down list.

Enabling the Chemically Activated Bimolecular Reaction option results in a net rate constant

at any pressure being defined as Equation . in the Theory Guide.

The parameters you specified under Arrhenius Rate in the Reactions dialog box represent

the high-pressure Arrhenius parameters. You can, however, specify values for the following

parameters under Low Pressure Arrhenius Rate:

ln(Pre-Exponential Factor)

(

in Equation . in the Theory Guide) The pre-exponential factor

is often an extremely

large number, so you will input the natural logarithm of this term.

(

in Equation . in the Theory Guide)

(

If you selected troe for the Reaction Type, you can specify values for Alpha, T1, T2, and T3

( ,

,

, and

in Equation . in the Theory Guide) under Troe parameters. If you selected

sri for the Reaction Type, you can specify values for a, b, c, d, and e ( ,

, ,

, and  in

Equation . in the Theory Guide) under SRI parameters.

Coverage Dependent Reaction

If you are modeling Wall Surface reactions with site-balancing and you have reaction rates that

depend on site coverages, you can enable the Coverage Dependent Reaction option. Click Specify...

to open the Coverage Dependent Reaction dialog box (Figure . :The Coverage Dependent

Reaction Dialog Box (p. )) and input the coverage parameters.

Figure . : The Coverage Dependent Reaction Dialog Box

In the Coverage Dependent Reaction dialog box, all the site species of the reaction will be

present with a default value of  for all the parameters, corresponding to no surface coverage

modification. Enter the relevant values of the parameters , , and  (as defined in Equa-

tion . in the Theory Guide) for all the species for which the reaction has coverage depend-

ence.

and  are dimensionless, and  is in units of J/kgmol.

. If you are using the laminar finite-rate, eddy-dissipation concept or PDF transport model for turbulence-

chemistry interaction, and the reaction is reversible, enable the Include Backward Reaction option for

the Arrhenius Rate.When this option is enabled, you will not be able to edit the Rate Exponent for

the product species, which instead will be set to be equivalent to the corresponding product Stoi-

ch. Coefficient. By default, ANSYS Fluent calculates the reverse reaction rate constants using Equa-

tion . in the Fluent Theory Guide.You can overwrite the ANSYS Fluent’s default parameters for the

reactions or define your own reactions. In both scenarios, you also need to specify the standard-state

enthalpy and standard-state entropy for mixture material. ANSYS Fluent will use these values in the

calculation of the backward reaction rate constant (Equation . in the Fluent Theory Guide).

In addition, you have the option to provide your own backward reaction parameters. To do this,

click Specify... next to Include Backward Reaction and enable the Arrhenius Backward Rate

option in the Backward Reaction Parameters dialog box that opens (see Figure . : Backward

Reaction Parameters Dialog Box (p. )).

Figure . : Backward Reaction Parameters Dialog Box

You can specify the following backward rate parameters:

in Equation . in the Fluent Theory Guide).

in the backward rate constant expression in Equation . in the Fluent Theory

Guide).

ANSYS Fluent will use your custom values to calculate the backward rate constant of the reversible

reaction according to Equation . in the Fluent Theory Guide.

Note that the reversible reaction option is not available for either the eddy-dissipation or the finite-

rate/eddy-dissipation turbulence-chemistry interaction model.

. If you are using the eddy-dissipation or finite-rate/eddy-dissipation model for turbulence-chemistry

interaction, you can enter values for A and B under the Mixing Rate heading.These values should not

be changed unless you have reliable data. In most cases you will use the default values.

A is the constant  in the turbulent mixing rate (Equation . and Equation . in the Theory

Guide) when it is applied to a species that appears as a reactant in this reaction. The default

setting of . is based on the empirically derived values given by Magnussen et al. [] (p. ).

B is the constant  in the turbulent mixing rate (Equation . in the Theory Guide) when it is

applied to a species that appears as a product in this reaction. The default setting of . is based

on the empirically derived values given by Magnussen et al. [] (p. ).

. Repeat steps – for each reaction you need to define. After defining all reactions, click OK.

..... Defining Species and Reactions for Fuel Mixtures

Quite often, combustion systems will include fuel that is not easily described as a pure species (such

as CH4 or C2H6). Complex hydrocarbons, including fuel oil or even wood chips, may be difficult to

define in terms of such pure species. However, if you have available the heating value and the ultimate

analysis (elemental composition) of the fuel, you can define an equivalent fuel species and an equi-

valent heat of formation for this fuel. Consider, for example, a fuel known to contain % C, % H,

and % O by weight. Dividing by atomic weights, you can arrive at a “fuel” species with the mo-

lecular formula C4.17H6O275. You can start from a similar, existing species or create a species from

nothing, and assign it a molecular weight of . kg/kmol (. +    + . ). The

chemical reaction would be considered to be

(.)

You will need to set the appropriate stoichiometric coefficients for this reaction.

The heat of formation (or standard-state enthalpy) for the fuel species can be calculated from the

known heating value

since

(.)

where

is the standard-state enthalpy on a molar basis. Note the sign convention in Equa-

tion . (p. ) :

is negative when the reaction is exothermic.

.... Defining Zone-Based Reaction Mechanisms

If your ANSYS Fluent model involves reactions that are confined to a specific area of the domain, you

can define “reaction mechanisms” to enable different reactions selectively in different geometrical

zones. You can create reaction mechanisms by selecting reactions from those defined in the Reactions

dialog box and grouping them. You can then assign a particular mechanism to a particular zone.

..... Inputs for Reaction Mechanism Definition

To define a reaction mechanism, click the Edit... button to the right of Mechanism. The Reaction

Mechanisms Dialog Box (p. ) (Figure . : The Reaction Mechanisms Dialog Box (p. )) will open.

Figure . : The Reaction Mechanisms Dialog Box

The steps for defining a reaction mechanism are as follows:

. Set the total number of mechanisms in the Number of Mechanisms field. Use the arrows to change

the value, or type the value and press Enter.

. Set the Mechanism ID of the mechanism you want to define. Again, if you type in the value, be sure

to press Enter.

. Specify the Name of the mechanism.

. Select the type of reaction to add to the mechanism under Reaction Type. If you select Volumetric,

the Reactions list will display all available fluid-phase reactions. If you select Wall Surface or Particle

Surface, the Reactions list will display all available wall surface reactions (described in Wall Surface

Reactions and Chemical Vapor Deposition (p. )) or particle surface reactions (described in Particle

Surface Reactions (p. )). If you select All, the Reactions list will display all available reactions.This

option is meant for backward compatibility with ANSYS Fluent . or earlier cases.

. Select the reactions to be included in the mechanism.

For Volumetric or Particle Surface reactions, select available reactions for the mechanism in the

Reactions list.

For Wall Surface reactions, use the following procedure:

a.

a.

Select available wall surface reactions for the mechanism in the Reactions list.

b. If any site species appear in the selected reaction(s), set the number of sites in the Number of

Sites field. Use the arrows to change the value, or type the value and press Enter. See Reaction-

Diffusion Balance for Surface Chemistry in the Theory Guide for details about site species in wall

c.

If you specify a Number of Sites that is greater than zero, specify the properties of the site.

Site Name

(optional)

Site Density

(in kmol/m2) This value is typically in the range of - to -.

Click the Define... button. This will open the Site Parameters Dialog Box (p. ) (Fig-

ure . : The Site Parameters Dialog Box (p. )), where you will define the parameters

of the site species.

Figure . : The Site Parameters Dialog Box

Site Name

is the optional name of the site that was specified in the Reaction Mechanisms dialog box.

Total Number of Site Species

is the number of adsorbed species that are to be modeled at the site. (Use the arrows to

change the value, or type the value and press Enter.)

Under Site Species, select the appropriate species from the drop-down list(s) and

specify the fractional Initial Site Coverage for each species. For steady-state calculations,

it is recommended (though not strictly required) that the initial values of Initial Site

Coverage sum to unity. For transient calculations, it is required that these values sum

to unity.

Click Apply in the Site Parameters dialog box to store the new values.

to unity.

. Repeat steps – for each reaction mechanism you need to define.When you are finished defining all

reaction mechanisms, click OK.

.... Defining Physical Properties for the Mixture

When your ANSYS Fluent model includes chemical species, the following physical properties must

be defined, either by you or by the database, for the mixture material:

density, which you can define using the gas law or as a volume-weighted function of composition

viscosity, which you can define as a function of composition

thermal conductivity and specific heat (in problems involving solution of the energy equation), which

you can define as functions of composition

mass diffusion coefficients and Schmidt number, which govern the mass diffusion fluxes (Equation .

and Equation . in the Theory Guide)

Detailed descriptions of these property inputs are provided in Physical Properties (p. ).

Important

Remember to click the Change/Create button when you are done setting the properties

of the mixture material. The properties that appear for each of the constituent species will

depend on your settings for the properties of the mixture material. If, for example, you

specify a composition-dependent viscosity for the mixture, you will need to define viscosity

for each species.

.... Defining Physical Properties for the Species in the Mixture

For each of the fluid materials in the mixture, you (or the database) must define the following phys-

ical properties:

molecular weight, which is used in the gas law and/or in the calculation of reaction rates and mole-fraction

inputs or outputs

standard-state (formation) enthalpy and reference temperature (in problems involving solution of the

energy equation)

viscosity, if you defined the viscosity of the mixture material as a function of composition

thermal conductivity and specific heat (in problems involving solution of the energy equation), if you

defined these properties of the mixture material as functions of composition

standard-state entropy, if you are modeling reversible reactions

thermal and momentum accommodation coefficients, if you have enabled the low-pressure boundary

slip model.

Important

Global reaction mechanisms with one or two steps inevitably neglect the intermediate

species. In high-temperature flames, neglecting these dissociated species may cause the

temperature to be overpredicted. A more realistic temperature field can be obtained by

increasing the specific heat capacity for each species. Rose and Cooper  [] (p. ) have

created a set of specific heat polynomials as a function of temperature.

The specific heat capacity for each species is calculated as

(.)

The modified

polynomial coefficients (J/kg-K) are provided in Table . : Modified Spe-

cific Heat Capacity (Cp) Polynomial Coefficients  (p. ).

Table . : Modified Specific Heat Capacity (Cp) Polynomial Coefficients

Coefficient

.76317e+

.93780e+

.35446e+

.22828e-

.18077e+

.27867e+

.76317e+

.93780e+

.35446e+

.22828e-

.18077e+

.27867e+

.58304e-

.64357e-

.46776e-

.20247e-

.86327e-

.38224e-

.14741e-

.59578e-

.89204e-

.12377e-

—

—

.56597e-

—

—

The Coal Calculator dialog box automates calculation and setting of the relevant input parameters

for the Species, Discrete-Phase (DPM) and Pollutant models associated with coal combustion. It is

available in the Species dialog box for the Species Transport model when the Eddy-Dissipation or

Finite-Rate/Eddy-Dissipation turbulence-chemistry option is selected. You can define up to three

coal streams in your simulation using the Number of Coal Streams entry box.

Figure . : The Coal Calculator Dialog Box

For each coal stream selected in the Coal Stream ID, you need to define the following properties:

. Coal Proximate Analysis, which is the mass fraction of Volatile, Fixed Carbon, Ash and Moisture in the

coal. ANSYS Fluent will normalize the mass fractions so that they sum to unity.

. Coal Ultimate Analysis, which is the mass fraction of atomic C, H, O, N and optionally S, in the Dry-Ash-

Free (DAF) coal. ANSYS Fluent will normalize the mass fractions so that they sum to unity.

. A choice of One-step or Two-step chemical mechanism.The one-step mechanism is,

(.)

The two-step mechanism involves oxidation of volatiles to CO in the first reaction and oxidation

of CO to CO2 in the second reaction:

(.)

The stoichiometric coefficients in Equation . (p. ) and Equation . (p. ) are calculated

from the ultimate and proximate analyses.

(.)

. An option to Include SO2.When this is enabled, an input for the atomic mass fraction of sulphur, S, appears

in the ultimate analysis frame.

. The Coal Particle Material Name. A DPM combusting-particle material will be created with this name.

The default name is coal-particle.

. The Coal As-Received HCV, where HCV denotes the Higher Calorific Value.

. Volatile Molecular Weight is the molecular weight of pure volatiles.

. The CO/CO2 Split in Reaction  Products can be used to specify the molar fraction of CO to CO2 in the

first reaction of Equation . (p. ).The default value of  implies that all carbon is reacted to CO, with

no CO2 produced.

. The High Temperature Volatile Yield. Enhanced devolatization at higher temperatures can cause the

volatile yield to exceed the proximate analysis fraction.To model this, the actual volatile fraction used is

calculated as that specified in the Proximate Analysis input multiplied by the High Temperature

Volatile Yield.The actual fixed carbon fraction is then calculated as one minus the sum of the actual

volatile, ash and moisture fractions.

. Fraction of N in Char (DAF).This input is used in calculating the split of atomic nitrogen for the Fuel

NOx model.

. Coal Dry Density is used to calculate the volume fraction of liquid-water for the Wet Combustion option

in the Injections dialog box.

Clicking Apply will save the Coal Property data for the selected Coal Stream ID. When you click OK,

ANSYS Fluent makes the following changes:

. A Mixture material is created, named coal-volatiles-air, with a one or two step reaction mechanism as

specified in the Mechanism option. If the Fluid material species (O2, CO, CO2, and so on) do not exist,

they are created. A Fluid material called coal-volatiles, is also created with a standard state enthalpy cal-

culated from the ultimate and proximate analyses, as-received HCV and volatile molecular weight. For

the second and third coal streams, additional Fluid materials and reactions with the properties corres-

ponding to the second and third coal streams are also created in the mixture.

. A combusting-particle material is created for each coal stream with Volatile Component Fraction and

Combustible Fraction calculated from the ultimate and proximate analyses.The discrete phase model

(DPM) is enabled.

. For the fuel NOx model, the default fuel species is set to vol, the char N conversion is set to NO, and the

fuel NOx  Volatile and Char mass fractions are set according to the ultimate and proximate compositions

of the first coal stream. Note that even though some of the default fuel NOx parameters are changed, the

fuel NOx model itself is not enabled.

. If the Moisture mass fraction in the coal proximate analysis is nonzero, then the Wet Combustion option

is enabled in the Coal Calculator dialog box, and all subsequent injections that are created will have wet

combustion enabled.The liquid material will be set to water-liquid, and the volume fraction of water

will be calculated from the Moisture mass fraction specified in the proximate analysis and the Coal Dry

Density.The wet combustion settings are not modified for existing injections.The Density for the com-

busting-particle in the Create/Edit Materials dialog box will also be set to Coal Dry Density.

Note

Irrespective of the Wet Combustion option in the Coal Calculator dialog box you can

modify the Wet Combustion model setting for the injections in the Set Injection Properties

dialog box. In addition, you will need to take care to enter the flow-rate of each injection

on a wet or dry basis, consistent with the Wet Combustion model setting.

You will need to specify the inlet mass fraction for all species in your simulation. In addition, for pressure

outlets you will set species mass fractions to be used in case of backflow. At walls, ANSYS Fluent will

apply a zero-gradient (zero-flux) boundary condition for all species by default, although you can change

each species boundary condition to a specified value. If you have surface reactions defined (see Wall

Surface Reactions and Chemical Vapor Deposition (p. )), you can choose to enable wall-surface reac-

tions and select the chemical mechanism. For fluid zones, you also have the option of specifying a

reaction mechanism. Input of cell zone and boundary conditions is described in Cell Zone and

Important

Non-reflecting boundary conditions (NRBCs) are not compatible with species transport models.

They are mainly used to solve ideal-gas single species flow. For information about NRBCs, see

Note that you will explicitly set mass fractions only for the first

species.The solver will

compute the mass fraction of the last species by subtracting the total of the specified mass

fractions from . If you want to explicitly specify the mass fraction of the last species, you must

reorder the species in the list (in the Create/Edit Materials Dialog Box (p. )), as described in

Defining Properties for the Mixture and Its Constituent Species (p. ).

.... Diffusion at Inlets with the Pressure-Based Solver

For the pressure-based solver in ANSYS Fluent, the net transport of species at inlets consists of both

convection and diffusion components. The convection component is fixed by the specified inlet

species mass or mole fraction, whereas the diffusion component depends on the gradient of the

computed species concentration field (which is not known a priori). At very small convective inlet

velocities, for example when modeling perforated combustion liners with an inlet, substantial mass

can be gained or lost through the inlet due to diffusion. For this reason, inlet diffusion is disabled by

default, but can be enabled with the Inlet Diffusion option in the Species Model dialog box.

Edit...

You can define a source or sink of a chemical species within the computational domain by defining a

source term in the Fluid dialog box. You may choose this approach when species sources exist in your

problem but you do not want to model them through the mechanism of chemical reactions. Defining

Mass, Momentum, Energy, and Other Sources (p. ) describes the procedures you would follow to

define species sources in your ANSYS Fluent model. If the source is not a constant, you can use a user-

defined function. See the Fluent Customization Manual for details about user-defined functions.

While many simulations involving chemical species may require no special procedures during the

solution process, you may find that one or more of the solution techniques noted in this section helps

to accelerate the convergence or improve the stability of more complex simulations. The techniques

outlined below may be of particular importance if your problem involves many species and/or chem-

ical reactions, especially when modeling combusting flows.

.... Stability and Convergence in Reacting Flows

Obtaining a converged solution in a reacting flow can be difficult for a number of reasons. First, the

impact of the chemical reaction on the basic flow pattern may be strong, leading to a model in which

there is strong coupling between the mass/momentum balances and the species transport equations.

This is especially true in combustion , where the reactions lead to a large heat release and subsequent

density changes and large accelerations in the flow. All reacting systems have some degree of coupling,

however, when the flow properties depend on the species concentrations. These coupling issues are

best addressed by the use of a two-step solution process, as described below, and by the use of under-

relaxation as described in Setting Under-Relaxation Factors (p. ).

A second convergence issue in reacting flows involves the magnitude of the reaction source term.

When the ANSYS Fluent model involves very rapid reaction rates (reaction time scales are much faster

than convection and diffusion time scales), the solution of the species transport equations becomes

numerically difficult. Such systems are termed “stiff” systems. Stiff systems with finite-rate chemistry

should be solved using either the pressure-based or density-based solver together with either Stiff

Chemistry Solver or the CHEMKIN-CFD Solver (see Solution of Stiff Chemistry Systems (p. )). Finite-

rate chemistry may also be used for turbulent combustion. For turbulent combustion, turbulence-

chemistry interactions can either be neglected (Finite-rate/No TCI model) or accounted for using

Eddy-Dissipation Concept or PDF Transport models.

....Two-Step Solution Procedure (Steady-state Only)

Solving a reacting flow as a two-step process is a practical method for reaching a stable converged

solution to your ANSYS Fluent problem. In this process, you begin by solving the flow, energy, and

species equations with reactions disabled (the “cold-flow”, or unreacting flow). When the basic flow

pattern has thereby been established, you can re-enable the reactions and continue the calculation.

The cold-flow solution provides a good starting solution for the calculation of the combusting system.

This two-step approach to combustion modeling can be accomplished using the following procedure:

. Set up the problem including all species and reactions of interest.

. Temporarily disable reaction calculations by turning off Volumetric in the Species Model Dialog

Box (p. ).

Edit...

. Disable calculation of the product species in the Equations Dialog Box (p. ).

Solution →

Controls → Equations...

. Calculate an initial (cold-flow) solution. (Note that it is generally not productive to obtain a fully converged

cold-flow solution unless the non-reacting solution is also of interest to you.)

. Enable the reaction calculations by turning on Volumetric again in the Species Model Dialog Box (p. ).

. Enable all equations in the Equations dialog box. If you are using the Finite-Rate/No TCI, Finite-

Rate/Eddy-Dissipation, Eddy-Dissipation Concept or PDF Transport model for the turbulence-

chemistry interaction, you may need to patch an ignition source (as described in Ignition in Steady-State

Combustion Simulations (p. )).

.... Density Under-Relaxation

One of the main reasons a combustion calculation can have difficulty converging is that large changes

in temperature cause large changes in density, which can, in turn, cause instabilities in the flow

solution. When you use the pressure-based solver, ANSYS Fluent allows you to under-relax the change

in density to alleviate this difficulty. The default value for density under-relaxation is , but if you

encounter convergence trouble you may want to reduce this to a value between . and  (in the

Solution Controls task page).

Note that if you are using a real-gas model the solution might converge at a slower rate than when

running ideal-gas flow. To improve the convergence performance of your analysis, you need to reduce

the underrelaxation for density to values as low as ..

.... Ignition in Steady-State Combustion Simulations

If you introduce fuel to an oxidant or have a premixed fuel/oxidant mixture, but you are not simulating

the transient ignition process, then you must numerically force the solution to the burned state (rather

than the unburned state). Generally, spontaneous ignition does not occur unless the temperature of

the mixture exceeds the activation energy threshold required to maintain combustion. For steady-

state ANSYS Fluent combustion simulations, whether you are using the species transport or PDF

transport model and regardless of turbulence-chemistry interaction option, you have to supply an

ignition source to initiate combustion. This ignition source may be a heated surface or inlet mass

flow that heats the gas mixture above the required ignition temperature. Often, however, it is the

equivalent of a spark: an initial solution state that causes combustion to proceed. You can supply this

initial “spark” by patching a hot temperature into a region of the ANSYS Fluent model that contains

an ignitable fuel/air mixture.

Solution →

Initialization → Patch...

Depending on the model, you may need to patch both the temperature and the fuel/ oxidant/product

concentrations to produce ignition in your model. The initial patch has no impact on the final steady-

state solution—no more than the location of a match determines the final flow pattern of the torch

that it lights. See Patching Values in Selected Cells (p. ) for details about patching initial values.

.... Solution of Stiff Chemistry Systems

When modeling stiff chemistry systems, such as flames with finite-rate kinetics, you can either use

the pressure-based solver with the Stiff Chemistry Solver option enabled or CHEMKIN-CFD Solver

selected as seen in the Species Model Dialog Box (p. ) (Figure . : The Species Model Dialog

Box (p. )), or the density-based solver.

For steady simulations using the pressure-based solver, the Stiff Chemistry Solver option approximates

the reaction rate

in the species transport equation (see Equation . in the Theory Guide) as,

(.)

where  is an appropriate time-step. Note that as  tends to zero the approximation becomes exact

but the stiff numerics will cause the pressure-based solver to diverge. On the other hand, as  tends

to infinity, the approximated reaction rate

tends to zero and, while the numerical stiffness is alle-

viated, there is no reaction. In ANSYS Fluent, the default value for  is set to one-tenth of the minimum

convective or diffusive time-scale in the cell. This value was found to be sufficiently accurate and robust,

although it can be modified using the solve/set/stiff-chemistry text command. ISAT is

employed to integrate the stiff chemistry in Equation . (p. ). Equation . (p. ) is also applied

for unsteady simulations, with  = flow time step.

Details about the ISAT algorithm may be found in Particle Reaction in the Theory Guide and Using

ISAT Efficiently (p. ). For efficient and accurate use of ISAT, a review of this section is highly recom-

mended.

mended.

The density-based implicit solver may also be used with either chemistry solver option. This option

allows a larger stable Courant (CFL) number specification, although additional calculations are required

to calculate the eigenvalues of the chemical system Jacobian [] (p. ). When enabling the stiff-

chemistry solver with the density-based solver, the following must be specified:

Temperature Positivity Rate Limit: limits new temperature changes by this factor multiplied by the old

temperature. Its default value is ..

Temperature Time Step Reduction: limits the local CFL number when the temperature is changing too

rapidly. Its default value is ..

.... Eddy-Dissipation Concept Model Solution Procedure

Due to the high computational expense of the Eddy-Dissipation Concept model, it is recommended

that you use the following procedure to obtain a solution using the pressure-based solver:

. Calculate an initial solution using the equilibrium Non-premixed or Partially-premixed model (see Mod-

eling Non-Premixed Combustion (p. ) and Modeling Partially Premixed Combustion (p. )).

. Import a CHEMKIN format reaction mechanism (see Importing a Volumetric Kinetic Mechanism in CHEMKIN

Format (p. )).

. Enable the reaction calculations by turning on Volumetric Reactions in the Species Model dialog box

and selecting Eddy-Dissipation Concept under Turbulence-Chemistry Interaction. Select the mech-

anism that you just imported as the Mixture Material.

Edit...

. Set the species boundary conditions.

Setup →

Edit...

Setup →

. Disable the flow and turbulence and solve for the species and temperature only.

. Enable all equations and iterate to convergence. Note that the default numerical parameters for the

solution of the Eddy-Dissipation Concept equations are set to provide maximum robustness with slowest

convergence.The convergence rate can be increased by setting the Aggressiveness Factor in the

Species dialog box or with the text command:

define → models → species → set-turb-chem-interaction

The Aggressiveness Factor can be set from  (slow but stable) to  (fast but least stable). The

default is .

ANSYS Fluent can report chemical species as mass fractions, mole fractions, and molar concentrations.

You can also display laminar and effective mass diffusion coefficients. The following variables are

available for postprocessing of species transport and reaction simulations:

Mass fraction of species-n

Mole fraction of species-n

Molar Concentration of species-n

Lam Diff Coef of species-n

Eff Diff Coef of species-n

Thermal Diff Coef of species-n

Enthalpy of species-n (pressure-based solver calculations only)

species-n Source Term (density-based solver calculations only)

TFM Thickening Factor (Thickened Flame Model only)

TFM Omega (Thickened Flame Model only)

TFM Thickening Factor (turbulent cases (LES / DES / SAS / SBES / SDES) with Thickened Flame Model only)

Laminar Flame Speed (Thickened Flame Model only)

Laminar Flame Thickness (Thickened Flame Model only)

Cell Time Scale (Eddy-Dissipation Concept and laminar finite-rate with stiff-chemistry only)

Fine Scale Mass fraction of species-n (Eddy-Dissipation Concept model only)

EDC Cell Volume Fraction (Eddy-Dissipation Concept model only)

Fine Scale Temperature (Eddy-Dissipation Concept model only)

Net Rate of species-n (Eddy-Dissipation Concept and laminar finite-rate with stiff-chemistry only)

Kinetic Rate of Reaction-n

Turbulent Rate of Reaction-n

Liquid species mass fraction of species-n (solidification and melting model only)

These variables are contained in the Species..., Temperature..., and Reactions... categories of the

variable selection drop-down list that appears in postprocessing dialog boxes. See Field Function

Definitions (p. ) for a complete list of flow variables, field functions, and their definitions. Displaying

Graphics (p. ) and Reporting Alphanumeric Data (p. ) explain how to generate graphics displays

and reports of data.

.... Averaged Species Concentrations

Averaged species concentrations at inlets and exits, and across selected planes (that is, surfaces that

you have created using Create in the Domain ribbon tab (Surfacegroup box)) within your model

can be obtained using the Surface Integrals Dialog Box (p. ), as described in Surface Integra-

tion (p. ).

Edit...

Select the Molar Concentration of species-n for the appropriate species in the Field Variable drop-

down list.

For gas-phase reactions, the reaction rate is defined on a volumetric basis and the rate of creation and

down list.

destruction of chemical species becomes a source term in the species conservation equations. Hetero-

geneous surface reactions create sources (and sinks) of chemical species in the gas-phase as well, but

also alter surface coverages for surface site reactions, and may deposit or etch species for bulk (solid)

reactions.

For more information about the theoretical background of wall surface reactions and chemical vapor

depositions, see Wall Surface Reactions and Chemical Vapor Deposition in the Theory Guide. Information

about using wall surface reactions is presented in the following subsections:

... Overview of Surface Species and Wall Surface Reactions

... Importing a Surface Kinetic Mechanism in CHEMKIN Format

... Manual Inputs for Wall Surface Reactions

... Including Mass Transfer To Surfaces in Continuity

...Wall Surface Mass Transfer Effects in the Energy Equation

... Modeling the Heat Release Due to Wall Surface Reactions

... Solution Procedures for Wall Surface Reactions

... Postprocessing for Surface Reactions

ANSYS Fluent treats chemical species adsorbed and desorbed, as well as those deposited into or etched

from the bulk solid surfaces as distinct from the same chemical species in the gas. Similarly, surface

reactions are defined distinctly and treated differently than gas-phase reactions involving the same

Surface reactions can be limited so that they occur on only some of the wall boundaries (while the

other wall boundaries remain free of surface reaction). The surface reaction rate is defined and computed

per unit surface area, in contrast to the fluid-phase reactions, which are based on unit volume.

Importing surface kinetic mechanisms in CHEMKIN format requires that the gas-phase mechanism file

accompanies the surface mechanism file for full compatibility with CHEMKIN (for more information on

how to import the gas-phase mechanism, see Importing a Volumetric Kinetic Mechanism in CHEMKIN

Format (p. )). If the gas-phase mechanism file is not available, then you will need to create one that

you will import along with the surface mechanism file.

The mechanism files are imported into ANSYS Fluent using the Import CHEMKIN Format Mechanism

dialog box (Figure . : The Import CHEMKIN Format Mechanism Dialog Box for Surface Kinetics (p. ))

which is opened by clicking Import CHEMKIN Mechanism... in the Species Model dialog box.

Wall Surface Reactions and Chemical Vapor Deposition

Figure . : The Import CHEMKIN Format Mechanism Dialog Box for Surface Kinetics

In the Import CHEMKIN Format Mechanism dialog box:

. Enable Import Surface Mechanism.

. Enter the paths in the Kinetic Input File text fields in the Gas-Phase and Surface group boxes (for example,

path/chem.inp and path/ path/surf.inp, respectively).

If you provide some or all species thermodynamic data in a separate file, disable All contained in Kin-

etics Input File and specify the thermodynamic data file location.

cpropep\data directory in your ANSYS Fluent installation area or specify the path of your ther-

modynamic database file if thermo.db does not contain all the gas-phase species in the CHEMKIN

mechanism. The format for thermo.db is detailed in the CHEMKIN manual  [] (p. ).

. To specify the surface species thermodynamic database, you can:

Select All contained in Kinetics Input File under the Thermodynamic Database  and include the

surface species thermodynamics data in the surface kinetics input file.

Select Same as 'Gas-Phase' and include the surface species thermodynamics data in the thermodynamics

data file used in the gas-phase mechanism. Note that the default thermo.db file contains only gas-

phase species. If you want to use this file, you will need to supply a thermodynamic database that includes

surface species defined in your simulation.

Note

The surface species thermodynamic data must be included either in the surface kinetics

input file or in the gas-phase thermodynamics data file. If you do not import thermody-

Note

namics data as a separate file in the gas-phase mechanism, then all surface thermody-

namics data must be contained in the surface kinetics input file.

ANSYS Fluent will create a material with the specified name, which will contain the CHEMKIN data for

the species and reactions, and add it to the list of Fluent Mixture Materials. You can view all of the

reactions by clicking the Edit... button to the right of Mechanism, under Properties in the Create/Edit

Materials Dialog Box (p. ).

ANSYS Fluent will also automatically save the imported data within the Fluent case file. Note that

carrying the original input files along with the Fluent case file is not required. ANSYS Fluent will auto-

matically retrieve these files when needed (for example, when using the CHEMKIN-CFD solver).

For details on importing gas species transport properties, see Procedure for Importing Volumetric

CHEMKIN Mechanisms (p. ).

Important

A surface reaction rate constant can be expressed in terms of a sticking coefficient in

CHEMKIN mechanisms. When Stiff Chemistry Solver is selected from the Chemistry Solver

drop-down list, ANSYS Fluent will convert this sticking coefficient form to an equivalent

Arrhenius rate expression [] (p. ). For full compatibility with ANSYS Chemkin-Pro, select

CHEMKIN-CFD Solver instead.

.... Compatibility and Limitations for Gas Phase Reactions

Generally, ANSYS Fluent handles all reaction types that are supported in ANSYS Chemkin-Pro. However,

some limitations still exist for the following models and features:

the None – Explicit Source chemistry solver (non-stiff chemistry)

the Finite-Rate/Eddy-Dissipation turbulence-chemistry interaction

In these cases, only the following volume reaction types can be used:

Arrhenius, including those reactions with arbitrary reaction order, third-body efficiencies and non-integer

stoichiometric coefficients

Pressure-dependent reactions using the Lindemann,Troe and SRI forms

CHEMKIN mechanism files with CHEMKIN-default rate parameter units

Duplicate reactions (keyword DUP)

Arbitrary reverse reaction (keyword REV)

.... Compatibility and Limitations for Surface Reactions

When using surface reactions in your simulation, note the following:

Surface reactions are not supported with the density-based solver.

As with volume reactions, ANSYS Fluent generally handles all reaction types that are supported in ANSYS

Chemkin-Pro. However, with the None – Explicit Source chemistry solver or Finite-Rate/Eddy-Dissipation

turbulence-chemistry interaction, only the following surface reaction types can be used:

– Arrhenius reactions, including those with arbitrary reaction order, third-body efficiencies and non-integer

– Sticking coefficients (keyword STICK). ANSYS Fluent converts these to an equivalent Arrhenius expression.

– Arbitrary reaction units

– Duplicate reactions (keyword DUP)

– Surface coverage modification (keyword COV)

For a detailed description of the keywords, see ANSYS Chemkin-Pro Input Manual.

The basic steps for setting up a problem involving wall surface reactions are the same as those

presented in Overview of User Inputs for Modeling Species Transport and Reactions (p. ) for setting

up a problem with only fluid-phase reactions, with a few additions:

. In the Species Model Dialog Box (p. ):

Edit...

a.

Enable Species Transport, select Volumetric and Wall Surface under Reactions, and specify the

Mixture Material. See Enabling Species Transport and Reactions and Choosing the Mixture Materi-

al (p. ) for details about this procedure, and Mixture Materials (p. ) for an explanation of the

mixture material concept.

b. (optional) If you want to model the heat release due to wall surface reactions, enable the Heat of

Surface Reactions option.

c.

(optional) If you want to include the effect of surface mass transfer in the continuity equation, enable

the Mass Deposition Source option.

d. To control the robustness and the convergence speed, enter a value between  and  for the Aggress-

iveness Factor. A value of  is the most robust, but results in the slowest convergence.The default

value for the Aggressiveness Factor is ..

e. (optional) If you are using the pressure-based solver and you want to include species diffusion effects

in the energy equation, enable the Diffusion Energy Source option. See Wall Surface Mass Transfer

Effects in the Energy Equation (p. ) for details.

f.

(optional, but recommended for CVD) If you want to model full multicomponent (Stefan-Maxwell)

f.

diffusion or thermal (Soret) diffusion, enable the Full Multicomponent Diffusion or Thermal Diffusion

option. See Full Multicomponent Diffusion (p. ) for details.

Setup →

Materials

Mixture properties include the following:

reactions

Important

You will find all species (including the solid/bulk and site species) in the list of Fluent Fluid

Materials. For a deposited species such as Si, you will need both Si(g) and Si(s) in the mater-

ials list for the fluid material type.

Note that the final gas-phase species named in the Selected Species list should be the car-

rier gas.This is because ANSYS Fluent will not solve the transport equation for the final

species. Note also that any reordering, adding or deleting of species should be handled with

caution, as described in Assigning the Last Species (p. ).

. Check and/or set the properties of the individual species in the mixture. (See Defining Properties for the

Mixture and Its Constituent Species (p. ).) Note that if you are modeling the heat of surface reactions,

you should be sure to check (or define) the formation enthalpy for each species.

. Set species boundary conditions.

Setup →

In addition to the boundary conditions described in Defining Cell Zone and Boundary Conditions

for Species (p. ), you will first need to indicate whether or not surface reactions are in effect on

each wall. If so, you will then need to assign a reaction mechanism to the wall. To enable the effect

of surface reaction on a wall, enable the Reaction option in the Species section of the Wall dialog

box.

Important

If you have enabled the global Low-Pressure Boundary Slip option in the Viscous

Model Dialog Box (p. ), the Shear Condition for each wall will be reset to No Slip

even though the slip model will be in effect. Note that the Low-Pressure Boundary

Slip option is available only when the Laminar model is selected in the Viscous Model

See Inputs at Wall Boundaries (p. ) for details about boundary condition inputs for walls. See

User Inputs for Porous Media (p. ) for details about boundary condition inputs for porous media.

In the surface reaction boundary condition described above, the effects of the wall normal velocity or

bulk mass transfer to the wall are not included in the computation of species transport. The momentum

of the net surface mass flux from the surface is also ignored because the momentum flux through the

surface is usually small in comparison with the momentum of the flow in the cells adjacent to the

surface. However, you can include the effect of surface mass transfer in the continuity equation by

activating the Mass Deposition Source option in the Species Model Dialog Box (p. ).

Species diffusion effects in the energy equation due to wall surface reactions are included in the normal

species diffusion term described in Treatment of Species Transport in the Energy Equation in the

If you are using the pressure-based solver, you can neglect this term by disabling the Diffusion Energy

Source option in the Species Model Dialog Box (p. ). For the density-based solvers, this term is always

included; you cannot disable it. Neglecting the species diffusion term implies that errors may be intro-

duced to the prediction of temperature in problems involving mixing of species with significantly dif-

ferent heat capacities, especially for components with a Lewis number far from unity. While the effect

of species diffusion should go to zero at Le = , you may see subtle effects due to differences in the

numerical integration in the species and energy equations.

The heat release due to a wall surface reaction is, by default, ignored by ANSYS Fluent. You can,

however, choose to include the heat of surface reaction by activating the Heat of Surface Reactions

option in the Species Model Dialog Box (p. ) and setting appropriate formation enthalpies in the

Edit Material Dialog Box (p. ).

As in all CFD simulations, your surface reaction modeling effort may be more successful if you start

with a simple problem description, adding complexity as the solution proceeds. For wall surface reac-

tions, you can follow the same guidelines presented for fluid-phase reactions in Solution Procedures

for Chemical Mixing and Finite-Rate Chemistry (p. ).

In addition, if you are modeling the heat release due to surface reactions and you are having conver-

gence trouble, you should try temporarily turning off the Heat of Surface Reactions and Mass Depos-

ition Source options in the Species Model Dialog Box (p. ).

If you are modeling surface site species, good estimates of the Initial Site Coverage will aid conver-

gence.

In addition to the gas-phase variables listed in Postprocessing for Species Calculations (p. ), for

surface reactions you can display/report the surface coverage as well as the deposition rate of the

solid species deposited on a surface. Select Surface Coverage of species-n, Surface Deposition Rate

of species-n, or Porous Deposition Rate of species-n in the Species... category of the variable selection

Important

For surface reactions involving porous media, you can display/report the surface reaction

rates using the Kinetic Rate of Reaction-n(Porous) in the Reactions... category of the

variable selection drop-down list.

As described in The Multiple Surface Reactions Model in the Theory Guide, it is possible to define multiple

particle surface reactions to model the surface combustion of a combusting discrete-phase particle. For

more information about the theoretical background of particle surface reactions, see Particle Surface

Reactions in the Theory Guide. Information about using particle surface reactions is provided in the

following subsections:

... User Inputs for Particle Surface Reactions

... Modeling Gaseous Solid Catalyzed Reactions

... Using the Multiple Surface Reactions Model for Discrete-Phase Particle Combustion

The setup procedure for particle surface reactions requires only a few inputs in addition to the procedure

for volumetric reactions described in Overview of User Inputs for Modeling Species Transport and Re-

actions (p. ) – Defining Other Sources of Chemical Species (p. ). These additional inputs are as

follows:

In the Species Model dialog box, enable the Particle Surface option under Reactions.

Edit...

Particle Surface Reactions

When you specify the species involved in the particle surface reaction, be sure to identify the surface species,

as described in Defining Properties for the Mixture and Its Constituent Species (p. ).

Important

You will find all species (including the surface species) in the list of Fluent Fluid Materials.

If, for example, you are modeling coal gasification, you will find solid carbon, C(s), in the

materials list for the fluid material type.

For each particle surface reaction, select Particle Surface as the Reaction Type in the Reactions dialog

box, and specify the following parameters (in addition to those described in Defining Reactions (p. )):

Diffusion-Limited Species

When there is more than one gaseous reactant taking part in the particle surface reaction, the diffusion-

limited species is the species for which the concentration gradient between the bulk and the particle

surface is the largest. See Figure . : A Reacting Particle in the Multiple Surface Reactions Model in the

Theory Guide for an illustration of this concept. In most cases, there is a single gas-phase reactant and

the diffusion-limited species does not need to be defined.

Catalyst Species

This option is available only when there are no solid species defined in the stoichiometry of the particle

surface reaction. In such a case, you will need to specify the solid species that acts as a catalyst for the

reaction.The reaction will proceed only on the particles that contain this solid species. See Using the

Multiple Surface Reactions Model for Discrete-Phase Particle Combustion (p. ) for details on defining

the particle surface species mass fractions.

Diffusion Rate Constant

(

Effectiveness Factor

(

The catalytic particle surface reaction option is enabled in ANSYS Fluent when Particle Surface is se-

lected as the Reaction Type in the Reactions Dialog Box (p. ) and there are no solid species in the

reaction stoichiometry. The solid species acting as a catalyst for the reaction is defined in the Reactions

dialog box. The catalytic particle surface reaction will proceed only on those particles containing the

catalyst species.

... Using the Multiple Surface Reactions Model for Discrete-Phase Particle

Combustion

When you use the multiple surface reactions model, the procedure for setting up a problem involving

a discrete phase is slightly different from that outlined in Steps for Using the Discrete Phase Mod-

els (p. ). The revised procedure is as follows:

. Enable any of the discrete phase modeling options, if relevant, as described in Physical Models for the

Discrete Phase Model (p. ).

. Specify the initial conditions, as described in Setting Initial Conditions for the Discrete Phase (p. ).

. Define the boundary conditions, as described in Setting Boundary Conditions for the Discrete Phase (p. ).

. Define the material properties, as described in Setting Material Properties for the Discrete Phase (p. ).

Important

You must select multiple-surface-reactions in the Combustion Model drop-down list

in the Create/Edit Materials dialog box before you can proceed to the next step.

. If you have defined more than one particle surface species, for example, carbon (C<s>) and sulfur (S<s>),

you will need to return to the Set Injection Properties dialog box (or Set Multiple Injection Properties

dialog box) to specify the mass fraction of each particle surface species in the combusting particle. Click

the Multiple Reactions tab, and enter the Species Mass Fractions.These mass fractions refer to the

combustible fraction of the combusting particle, and should sum to . If there is only one surface species

in the mixture material, the mass fraction of that species will be set to , and you will not specify anything

under Multiple Surface Reactions.

. Set the solution parameters and solve the problem, as described in Solution Strategies for the Discrete

Phase (p. ).

. Examine the results, as described in Postprocessing for the Discrete Phase (p. ).

Important

Solid deposition reactions on the particle are not allowed together with custom laws.

Similar to wall surface reactions, electrochemical reactions generate sources (and sinks) in chemical

species transport equations.

For more information about the theoretical background of electrochemical reactions, see Electrochem-

ical Reactions in the Fluent Theory Guide. Information about using electrochemical reactions is presented

in the following sections:

... Overview of Electrochemical Reactions

... User Inputs for Electrochemical Reactions

... Electrochemical Reaction Effects in the Energy Equation

... Electrochemical Reaction Effects in the Species Transport Equation

... Including Mass Transfer in Continuity

... Solution Procedures for Electrochemical Reactions

An electrochemical reaction occurs only on wall surfaces where the electrolyte and the electrode meet.

Both aqueous and solid species can participate in electrochemical reactions. Solid species that can be

involved in electrochemical reactions are corroded or deposited species.

Electrochemical reactions can be limited so that they can only occur on some of the wall boundaries

(while the other wall boundaries remain free of reaction). The reaction rate is defined and computed

Electrochemical Reactions

You can specify different reaction mechanisms for different walls. Each reaction mechanism can have

multiple electrochemical reactions.

The steps needed to incorporate electrochemical reactions in your problem are as follows:

. For unsteady simulations, select Transient from the General task page (Solver group).

. Enable chemical species transport model.

Edit...

Figure . : The Species Model Dialog Box with Electrochemical Reactions Enabled

a.

In the Species Model dialog box, under Model, enable Species Transport.

b. Under Reactions, select Volumetric and Electrochemical.

Note

Once you enable the Electrochemical reactions, the electric potential solver will be

automatically enabled (under the Models tree branch).

. In the Create/Edit Materials dialog box, define all the species materials that are present in the electrolyte

and electrodes.

Setup →

Materials

a.

Copy the new species from the Fluent database to your case as described in Copying Materials from

the ANSYS Fluent Database (p. ). If your species material is not present in the database, copy a

similar species material and edit its properties, including Name and Chemical Formula.

Note

When copying species (including corroded and deposited solid species), make sure that

fluid is selected as Material Type in the Fluent Database Materials dialog box.

It is not necessary to represent the electron in the reaction, and e- can be safely ignored.

b. Under the Properties group box, set Charge Number for the new species.

Important

By default, Charge Number is set to , which means that the species is neutral. Make

sure to specify the Charge Number for all relevant species.

Note

Do not specify Electrical Conductivity for individual species. You will specify Elec-

trical Conductivity for the mixture.

. Edit the mixture composition using the Species dialog box (opened by clicking Edit next to Mixture

Species under Properties of the Create/Edit Materials dialog box).

a.

Remove unused species and add the electrochemical species to the Selected Species list as described

in Adding Species to the Mixture (p. ).

b. If solid species are involved in the electrochemical reactions (for example, in corrosion or electroplating

simulations), add them to the Selected Solid Species list.

Note

Make sure that the bulk species is the last species in the Selected Species list. ANSYS

Fluent solves transport equations for all but the last species in the Selected Species

list. The order of the solution is the same as the order of the species in Selected

Species.

. Specify the reactions in the Reactions dialog box (opened by clicking Edit next to Reactions under

Properties of the Create/Edit Materials dialog box).

For each reaction, configure the following settings:

a.

Select Electrochemical as the reaction type.

b. If you want the Tafel Equation . in the Fluent Theory Guide, rather than the Bulter-Volmer Equa-

a.

tion ., to be used in the kinetics calculation, select Tafel Parameters.

c.

Specify the following Butler-Volmer/Tafel Parameters:

Butler-Volmer parameters (the Tafel Parameters check box is cleared):

– Anodic Transfer Coefficient (

in Equation . in the Fluent Theory Guide)

– Cathodic Transfer Coefficient (

Tafel parameters (the Tafel Parameters check box is selected):

– Anodic Tafel Slope (

– Cathodic Tafel Slope (

Exchange Current Density (  in Equation . in the Fluent Theory Guide)

Equilibrium Potential (

You can define a constant, polynomial, piecewise-linear, or user-defined function for any of

the aforementioned Butler-Volmer/Tafel parameters.

d. Enter the

th species dimensionless power (

in Equation . in the Fluent Theory Guide) as Rate

Exponent.

e. Under the Butler-Volmer/Tafel Parameters group box, click the Specify Reference Mass Fractions...

button and in the Reference Mass Fractions dialog box that opens, enter the reference species mass

fractions (

Note

You can customize the electrochemical reaction rate by using the followoing UDFs:

DEFINE_EC_KINETICS_PARAMETER: to customize an individual kinetics parameter

in the Butler-Volmer reaction rate

DEFINE_EC_RATE: to define a totally different function form for the reaction rate.

Refer to DEFINE_EC_KINETICS_PARAMETER and DEFINE_EC_RATE in the

Fluent Customization Manual for details about those functions.

. Define reaction mechanisms using the Reaction Mechanisms dialog box (opened by clicking Edit next

to Mechanism under Properties of the Create/Edit Materials dialog box).

a.

Specify Number of Mechanisms. If you type in the value, be sure to press Enter.

b. For each electrochemical reaction mechanism, configure the following settings:

i.

Set the Mechanism ID of the mechanism you want to define. Again, if you type in the value, be

sure to press Enter.

ii.

Select Electrochemical as a reaction type.

iii. Under Reactions, select the reaction and in the Name text entry field, specify a meaningful name

for the mechanism (for example, mechanism-anode or mechanism-cathode).

. In the Create/Edit Materials dialog box, set the remaining mixture properties, such as Density (typically

volume-weighted-mixing-law), Mass Diffusivity, and Electrical Conductivity.

Note that if the anode, cathode, and electrolyte have different material properties, such as species

mass diffusivities, it is best to use a UDF. Alternatively, you can create new materials for the anode

and cathode by copying existing materials from the Fluent database, renaming them, and then

assigning these materials to the anode and cathode fluid zones in the Cell Zone Conditions dialog

box.

. For electrolyte and electrode zones, set cell zone conditions using Cell Zone Conditions Task Page (p. ).

Setup →

a.

In the Fluid dialog box, specify whether or not the selected zone is an electrolyte zone by selecting

Setup →

a.

or clearing the Electrolyte check box. By default, all fluid zones are electrolyte zones.

b. If there is no volumetric reactions, clear the Reaction check box.

. Set the electrochemical boundary conditions for all relevant walls using Boundary Conditions Task

Page (p. ).

Setup →

Figure . : Wall Potential Boundary Condition

Electrochemical reaction can be defined at either exterior (-sided) walls or interior (-sided) walls

with only one side exposed to electrolyte.

In the Wall dialog box, configure the following settings:

a.

For exterior (-sided) walls, set the potential boundary conditions as described in Using the Electric

Potential Model (p. ).

b. Specify whether or not the wall is Faradaic by selecting or clearing the Electrochemical Reaction

check box.

c.

For Faradaic walls, from the Reaction Mechanism drop-down list, select the reaction mechanism that

you have previously defined.

d. If the electrochemical reaction is defined on the wall (Electrochemical Reaction is selected), you can

include the reaction heat in the energy equation by selecting the Faradaic Heat check box.

Note

For the -sided wall, you need to specify the potential boundary conditions only on one

side of the wall. The settings you have specified will be automatically copied to the

other side of the wall.

. (optional) You can include additional sources in the energy, continuity, and species transport equations

as described in the following sections:

Electrochemical Reaction Effects in the Energy Equation (p. )

Electrochemical Reaction Effects in the Species Transport Equation (p. )

Including Mass Transfer in Continuity (p. ).

. Set the solution parameters in the Solution Methods Task Page (p. ) and Solution Controls Task

Page (p. ).

In many electrochemical applications, fluid convection can be neglected, in which case the Flow

equation should be disabled in the Equations control box (accessible from the Solution Controls

Similarly, for isothermal simulations, the Energy equation should be disabled.

Important

If the potential equation has difficulty converging, you can lower the Faradaic Interface

Current under-relaxation factor in the Solution Controls task page to improve stability.

. Once the solution is converged, you can display or report the following variables that are available under

the Potential category:

Electric Conductivity

Current Density

Total Echem Heat Source

In addition, you can display

Echem Reaction Rate of each reactions (under the Reactions category)

Surface Corrosion Rate of each solid species on a wall (under Species category)

When the electrochemical reaction model is enabled, you can specify two extra sources in the energy

equation:

Joule heating in the fluid and solid zones

You can include the Joule heating in the energy equation calculation by selecting the Include Joule

Heating in Energy Equation option in the Electric Potential dialog box (Using the Electric Potential

Electrochemical reaction heat at Faradaic interfaces

You can include the electrochemical reaction heat by selecting the Faradaic Heat option in the

boundary condition dialog boxes for each reacting wall.

When the electrochemical reaction model is enabled, you can specify an extra source in the species

transport equation for the ion-species:

Species migration in the electric field

You can include this effect by selecting the Species Migration option in the Species Model Dialog

Box (p. ).

When a solid species (corroded or deposited) is involved in an electrochemical reaction, the solid ma-

terial can enter or leave the flow domain. Usually the mass transfer of the solid species is small and

can be ignored in the continuity equation. However, if you want, you can include the mass source in

the continuity equation by using the following Scheme command:

(rpsetvar ‘potential/corrosion-source-in-continuity? #t)

The strongly nonlinear coupling between species and electric field can cause convergence problems.

To improve the stability of the solution, you can lower the Faradaic Interface Current under-relaxation

factor in the Solution Controls Task Page (p. ).

In addition, you can try temporarily disabling the Include Joule Heating in Energy Equation and

Faradaic Heat options (see Electrochemical Reaction Effects in the Energy Equation (p. )).

You can enable these options once the solution becomes more stable.

In addition to the volumetric and surface reactions described in the previous sections, you can also use

ANSYS Fluent to solve a species mixing problem without reactions. The species transport equations

that ANSYS Fluent will solve are described in Volumetric Reactions in the Theory Guide, and the procedure

you will follow to set up the non-reacting species transport problem is the same as that described in

Overview of User Inputs for Modeling Species Transport and Reactions (p. ) – Defining Other Sources

of Chemical Species (p. ), with some simplifications.

The basic steps are listed below:

. Enable Species Transport in the Species Model dialog box and select the appropriate Mixture Material.

Species Transport Without Reactions

Edit...

See Overview of User Inputs for Modeling Species Transport and Reactions (p. ) for information

about the mixture material concept, and Enabling Species Transport and Reactions and Choosing

the Mixture Material (p. ) for more details about using the Species Model dialog box.

. (optional) If you want to model full multicomponent (Stefan-Maxwell) diffusion or thermal (Soret) diffusion,

enable the Full Multicomponent Diffusion or Thermal Diffusion option.

. Check and/or define the properties of the mixture and its constituent species.

Setup →

Materials

Setup →

Materials

See Defining Properties for the Mixture and Its Constituent Species (p. ) for details.

. Set species boundary conditions, as described in Defining Cell Zone and Boundary Conditions for Spe-

cies (p. ).

No special solution procedures are usually required for a non-reacting species transport calculation.

Upon completion of the calculation, you can display or report the following quantities:

Concentration of species-n

Relative Humidity (when the water vapors (H2O) is present in the species mixture material)

These variables are contained in the Species... and Properties... categories of the variable selection

drop-down list that appears in postprocessing dialog boxes. See Field Function Definitions (p. ) for

a complete list of flow variables, field functions, and their definitions. Displaying Graphics (p. ) and

Reporting Alphanumeric Data (p. ) explain how to generate graphics displays and reports of data.

Information about using the reacting channel model is presented in the following subsections. For more

information about the theoretical background, see Reacting Channel Model in the Theory Guide.

... Overview and Limitations of the Reacting Channel Model

... Enabling the Reacting Channel Model

... Boundary Conditions for Channel Walls

... Postprocessing for Reacting Channel Model Calculations

The reacting channel model in ANSYS Fluent offers an efficient solution methodology for solving reacting

flow in shell and tube heat exchangers with long and thin channels. The volume inside the reacting

channels is not meshed and solved with the outer flow. Instead, a plug flow approximation is used for

the reacting channels, which is coupled to the outer flow through heat transfer across the channel

walls.

The reacting channel model has the following limitations:

The reacting channel model is available only for steady-state 3D problems.

The reacting channel model solves the one-dimensional species equations at the centerline of the reacting

channel.The accuracy of the model depends on how well ANSYS Fluent computes the channel centerline

from the channel wall surface mesh. It is highly recommended to use a swept structured surface mesh on

the channel wall (see Figure . : Optimal Surface Mesh on the Reacting Channel Wall (p. )). Unstructured

channel wall surface meshes may result in loss of accuracy due to inconsistent channel centerlines.

Figure . : Optimal Surface Mesh on the Reacting Channel Wall

The steps and procedure to set up a reacting channel model are outlined below. In this section, the

steps pertinent to the reacting channel model only are explained. The setting up of other models used

in conjunction with reacting channel models are explained in other sections of the User's Guide.

. Enable the reacting channel model.

Reacting Channel Model

Setup → Models → Species → Reacting Channel Model

Edit...

Figure . : The Reacting Channel Model Dialog Box

When you enable the Enable Reacting Channel Model option, the dialog box will expand to show

the relevant inputs (see Figure . : The Reacting Channel Model Dialog Box (p. )).

. Specify the Number of Boundary Groups. If you have multiple channels, you can group together channels

with common flow direction, mixture materials, inlet compositions, temperature, pressure, and mass flow

rate.You will be required to provide the inputs for each boundary group.

Note

If you have multiple tubes, you will need to define each tube as a different wall and set

up the model by grouping the walls together if they have the same boundary conditions.

. Enter the number of Flow Iterations Per Coupling Iteration.This is the number of outer flow iterations

for each channel flow iteration.

. Optionally change an Under-Relaxation Factor.The value of the under-relaxation factor is used to update

the heat flux from the reacting channel. See Equation . in the Theory Guide.

. Set the Group Index. Note that the Group Index for the first boundary group is set to .

The inputs for each boundary group are entered in the Group Settings and Group Inlet Conditions

tabs as further described.

. Under the Group Settings tab, specify the model settings and options. (see Figure . :The Reacting

Channel Model Dialog Box (Group Inlet Conditions Tab) (p. )).

a.

a.

In the Channel Walls in Group selection list, select the wall boundary zones that correspond to the

reacting channels.

b. Select the group material from the Material drop-down list.You can choose any mixture material

available in the case as a group material.

c.

Optionally, import a CHEMKIN mechanism using Import CHEMKIN Mechanism... button. For details

see Importing a Volumetric Kinetic Mechanism in CHEMKIN Format (p. ).

d. To model surface reactions within the channel, enable Surface Reactions under Model Options group

box.The dialog box will expand to show the related inputs as shown in Figure . :The Reacting

Channel Model Dialog Box (p. ).These inputs include:

Surface to Volume Ratio of the channel group

Surface reaction mechanism of the group (selected from the Reaction Mechanism drop-down list)

e. To model porous medium, enable Porous Medium under Model Options group box.The dialog box

will expand to show porous medium inputs as shown in Figure . :The Reacting Channel Model

Dialog Box (p. ).These inputs include:

Porosity of the channel

Viscous Resistance in axial direction of the channel

Inertial Resistance in axial direction of the channel

Solid material of the porous medium inside the channel (selected from the Solid Material drop-

down list)

. Under the Group Inlet Conditions tab, specify the inlet conditions for the boundary group (see Fig-

ure . :The Reacting Channel Model Dialog Box (Group Inlet Conditions Tab) (p. )).You can specify

the inlet condition parameters as constant values. ANSYS Fluent provides you also with the option of re-

defining any or all of the inlet condition parameters using user-defined functions (UDFs).

Figure . : The Reacting Channel Model Dialog Box (Group Inlet Conditions Tab)

a.

Specify the X-, Y-, and Z-component of the flow at the inlets of the channels in the current group in

the Flow Direction group box.

Note

Since there is no surface or zone to identify the channel inlet or outlet, the inlet flow

direction of the group is used to determine the channel inlet. Therefore, It is very

important to specify the flow direction correctly.

b. Enter the inlet channel Temperature, Flow Rate and Pressure in the group.

c.

Specify the inlet mass fractions for each species in the group in the Species Composition group box.

d. To specify an inlet condition using a user-defined function (UDF), select the User Defined Inlet Con-

ditions check box and then select the appropriate user-defined function from the drop-down list. For

information about specifying and hooking DEFINE_REACTING_CHANNEL_BC UDFs, see

DEFINE_REACTING_CHANNEL_BC in the Fluent Customization Manual.

. Click the Apply button to save the settings.

. If you specified more than one boundary group in step , change the group ID value in Group Index integer

number entry box and repeat steps – for each remaining boundary group.

Once the reacting channel model is defined, you can generate reports or plots of reacting channel

variables using the Reacting channel 2D Curves dialog box (Figure . : Reacting Channel 2D Curves

Dialog Box (Plot) (p. )). You can open the Reacting channel 2D Curves dialog box by clicking the

Display Reacting Channel Variables button in the Reacting Channel Model dialog box. For inform-

ation about the plotting of reacting channel model variables, see Postprocessing for Reacting Channel

Model Calculations (p. ).

Modeling Curvilinear Reacting Channels

In the reacting channel model, the two ends of a channel are identified as the inlet and the outlet

based on the inputs provided for the inlet flow direction of the group. However, for some special

channel configurations, such as U-tubes, it is not possible to identify the inlet/outlet of the channel

based on the information of the inlet flow direction. For such cases, an additional input is required to

differentiate between the end points of the channel as inlet or outlet. The additional input is to provide

the centroid coordinates of the inlet of the U shaped channel. Therefore, for U-tube configurations,

after setting up the reacting channel model following the earlier steps in this section, it is required to

use the following text user interface commands to set the inlet and outlets correctly:

/define/models/species> reacting-channel-model-options

Are any of the channels a U-tube configuration? [no] yes

Is wall tube1 a U-tube configuration? [no] yes

Enter the coordinates of the center of the inlet for wall tube1

X coordinate [] .

Y coordinate []

Z coordinate []

Where tube1 is a reacting channel wall having a U shape. You will be asked the same questions for

each of the existing reacting channel walls.

In the ANSYS Fluent wall boundary conditions dialog box, the wall surfaces that you selected as

channel walls in the Reacting Channel Model dialog box will have zero heat flux boundary conditions,

which are disabled as shown in Wall Surface Reactions and Chemical Vapor Deposition (p. )).

Figure . : The Wall Boundary Condition Dialog Box for the Reacting Channel Model

The heat flux at the channel walls is calculated internally through the coupling of the reacting channel

model with the outer flow as described in Reacting Channel Model in the Theory Guide. For all other

wall surfaces, which are not channel walls, all boundary conditions as described in Wall Boundary

Conditions (p. ) are applicable.

ANSYS Fluent provides postprocessing options for plotting and reporting channel variables using the

Reacting Channel 2D Curves dialog box that opens by clicking the Display Reacting Channel Vari-

ables button in the Reacting Channel Model dialog box. You can generate X-Y plots or reports of

the following reacting channel variables:

Bulk mean temperature of the channel

Wall temperature of the channel

Nusselt Number (for the channel wall on the channel side)

Wall heat flux through the channel walls

Velocity inside the channel

Density of the channel

Mass fraction of the species inside the channel

The surface coverage and the deposition rate of the surface species.

The steps for generating the plots/reports are as follows:

.

Select either Plot Reacting Channel Variables or Report Reacting Channel Outlet Average.

The Reacting Channel 2D Curves dialog box displays either the Variable Name drop-down list

for selecting a single species for X-Y plot generation, or the Variable Names selection list for se-

lecting multiple species for report generation as shown in Figure . : Reacting Channel 2D

Curves Dialog Box (Plot) (p. ) and Figure . : Reacting Channel 2D Curves Dialog Box (Re-

port) (p. ).

Figure . : Reacting Channel 2D Curves Dialog Box (Plot)

Figure . : Reacting Channel 2D Curves Dialog Box (Report)

.

Specify whether you want to write the plot data to a file by using the Write To File check box.

.

If more than one boundary group is defined for reacting channel model, specify the group ID in the

Group Index integer number entry box.

.

The Variable Name drop-down/Variable Names selection list contains reacting channel variables of

the specified boundary group. Select the reacting channel variable(s) from the list.

.

Select the wall surface(s) from the Wall Surfaces selection list on which the plot/report will be generated

(at least one wall surface must be selected).

.

Click one of the following as applicable:

Plot to view X-Y plot in the graphics window

Print to view report in the console window

Write... to save to file

Information about using the Reactor Network model is presented in the following subsections.

... Overview and Limitations of the Reactor Network Model

... Solving Reactor Networks

... Postprocessing Reactor Network Calculations

For more information about the theoretical background, see Reactor Network Model in the Fluent Theory

Guide.

The Reactor Network model allows rapid solution of combustors using detailed chemical kinetic

mechanisms. This speed is achieved by first performing a Fluent CFD simulation with a fast chemistry

model, such as a Non-Premixed, Partially-Premixed, or Eddy-Dissipation model, and then using the

Reactor Network model to solve with a detailed kinetic mechanism. The Reactor Network model ag-

glomerates cells from the CFD solution into a user-specified small number of reactors and computes

detailed chemistry on this reactor network.

Since the chemical kinetics is decoupled from the flow, reactor network simulations are applicable to

steady simulations where the chemical kinetics does not affect the flow significantly, such as pollutant

formation. Inherently unsteady simulations, such as ignition and global extinction, cannot be modeled

with reactor networks. Note that the Reactor Network model can be used for unsteady simulations of

statistically steady flows, such as LES, where the time-averaged flow and species fields are used to

construct the reactor network.

The steps and procedure for setting up and solving a Reactor Network model are outlined below.

. Enable the Reactor Network model.

Setup → Models → Species → Reactor Network

Edit...

Important

Note that this model is only available when one of the reacting species models is enabled.

When you select the Reactor Network Model option, the dialog box expands to show the relevant

modeling controls (see Figure . : Reactor Network Dialog Box (Steady-State Flow) (p. )).

Reactor Network Model

Figure . : Reactor Network Dialog Box (Steady-State Flow)

. If a detailed chemical mechanism has already been imported, select the mixture material from the Detailed

Mechanism Material Name drop-down list. Otherwise import a mechanism in CHEMKIN format by

clicking Import CHEMKIN Mechanism....The mechanism files are imported into your case using the Import

CHEMKIN Format Mechanism dialog box as described in Specifying a Chemical Mechanism File for

Flamelet Generation (p. ).

. Set the Number of Reactors in the reactor network.The default value of  is a good starting value, but

it can be increased for greater accuracy.

. Specify whether or not the temperature is calculated from the equation of state by selecting or clearing

the Solve Temperature check box. By default, this option is selected, and ANSYS Fluent will determine

the temperatures in the reactor network.

. Once cells are agglomerated and a reactor-network solution is calculated, you can select the Use Current

Reactor Network option to perform further reactor network simulations with the existing network of

connected reactors.This option can be used to continue iterations from the previous reactor- network

solution if additional convergence is desired.The option also allows you to change the chemical mechanism

or species boundary conditions to generate a new solution on the current reactor network.

. (for transient analysis with the Data Sampling For Time Statistics option selected in the Run Calculation

task page only) Specify whether or not you want to use the time-averaged composition fields to agglom-

erate the reactors and time-averaged velocity fields to calculate the reactor mass flux matrix (instead of

the instantaneous fields) by selecting or clearing the Use Time Averaged Fields option.

Note

The Use Time Averaged Fields option should be used for unsteady simulations (for

example, LES) of statistically stationary combustors.

. If necessary, specify custom-field functions and adjust the default solver settings using the Expert Options

control.When Expert Options is selected, the Reactor Network dialog box expands to reveal the following

advanced options:

Figure . : Reactor Network Dialog Box - Expert Options

ODE Relative Error Tolerance, ODE Absolute Error Tolerance

The default values for the ODE relative and absolute error tolerances are 1e- and 1e-, respectively.

If the ODE solver fails to converge, it is often helpful to lower the ODE Relative Error Tolerance and

the ODE Absolute Error Tolerance.

Reactor Network Convergence Tolerance

The default value for the reactor network convergence tolerance is 1e-. Residuals should be well

converged at the default tolerance. Higher tolerances may be acceptable for engineering accuracy.

Solver

Solver

The default segregated solver typically converges faster than the coupled solver. However, when using

the segregated solver, residuals may stall above an acceptable tolerance. In this case, the coupled

solver should be used.

Maximum Number of Iterations (segregated solver)

If residuals are still decreasing and better convergence is desired, increase the maximum number of

iterations. If residuals are stalled and a quicker exit from the solver is desired, decrease the maximum

number of iterations.

Maximum Integration Time (coupled solver)

The ODE solver terminates the calculation at this time if residuals fail to converge.

Use Custom Field Functions to Define Reactor Zones

When selected, this option allows you to use custom field functions (Custom Field Functions (p. ))

as composition variables to create the reactor volumes. ANSYS Fluent clusters CFD cells that have

similar compositions using the following default composition variables:

temperature and mixture fraction for Non-Premixed and Partially-Premixed cases

temperature and mass fractions of N2 and H2O for Species Transport cases

You can override these default composition variables by selecting Use Custom Field Functions to

Define Reactor Zones and then selecting up to four custom field functions from the Custom Field

Functions selection list. ANSYS Fluent will group CFD cells that are close in these custom field function

composition variables. In the example shown in Figure . : Reactor Network Dialog Box - Expert

Options (p. ), cells with similar turbulent kinetic energy, x coordinate, and y coordinate will be ag-

glomerated to form the reactor network.

. Click Calculate Reactor Network to obtain a flow solution.

As the calculation is progressing, ANSYS Fluent prints the reactor network residuals for each iteration

Note

The reactor network solution should converge with the default settings. However, if the

model fails to converge with sufficient accuracy, you can adjust the default reactor

network solver settings by using the Expert Options control.

ANSYS Fluent provides additional postprocessing options for reactor network calculations. The following

reactor network variables are available for generating graphical plots:

Reactor Net Mass fraction of species-n

These variables will appear under the Reactor Network… postprocessing category of the variable

selection drop-down lists.

Chapter : Modeling Non-Premixed Combustion

This chapter provides details about the non-premixed combustion modeling capabilities in ANSYS Fluent.

The non-premixed combustion model is presented in the following sections:

.. Steps in Using the Non-Premixed Model

.. Setting Up the Equilibrium Chemistry Model

.. Setting Up the Steady and Unsteady Diffusion Flamelet Models

.. Defining the Stream Compositions

.. Setting Up Control Parameters

.. Calculating the Flamelets

.. Calculating the Look-Up Tables

.. Standard Files for Diffusion Flamelet Modeling

.. Setting Up the Inert Model

.. Defining Non-Premixed Boundary Conditions

.. Defining Non-Premixed Physical Properties

.. Solution Strategies for Non-Premixed Modeling

.. Postprocessing the Non-Premixed Model Results

For theoretical background on the non-premixed combustion model, see Non-Premixed Combustion

A description of the inputs for the non-premixed model is provided in the sections that follow.

... Preliminaries

... Defining the Problem Type

... Overview of the Problem Setup Procedure

Before turning on the non-premixed combustion model, you must enable turbulence calculations in

the Viscous Model Dialog Box (p. ).

Edit...

If your model is non-adiabatic, you should also enable heat transfer (and radiation, if required).

ON

Edit...

Figure . : Reacting Systems Requiring Non-Adiabatic Non-Premixed Model Approach in the Theory

Guide illustrates the types of problems that must be treated as non-adiabatic.

Your first task is to define the type of reaction system and reaction model that you intend to use. This

includes selection of the following options:

Non-premixed or partially premixed model option (see Modeling Partially Premixed Combustion (p. )).

Equilibrium chemistry model, steady diffusion flamelet model, unsteady diffusion flamelet model, or diesel

unsteady flamelet.

Adiabatic or non-adiabatic modeling options (see Non-Adiabatic Extensions of the Non-Premixed Model

Addition of a secondary stream (equilibrium model only).

Empirically defined fuel and/or secondary stream composition (equilibrium model only).

You can make these model selections using the Species Model dialog box (Figure . : The Species

Model Dialog Box (Chemistry Tab) (p. )).

Edit...

For a single-mixture-fraction problem, you will perform the following steps:

. Choose the chemical description of the system: chemical equilibrium, steady diffusion flamelet, unsteady

diffusion flamelet, or diesel unsteady flamelet (Figure . : Defining Equilibrium Chemistry (p. )).

. Indicate whether the problem is adiabatic or non-adiabatic.

Figure . : Defining Equilibrium Chemistry

Modeling Non-Premixed Combustion

. (steady diffusion flamelet model only) Import a flamelet file or appropriate CHEMKIN mechanism file if

generating flamelets (Figure . : Defining Steady Diffusion Flamelet Chemistry (p. )).

Figure . : Defining Steady Diffusion Flamelet Chemistry

. Define the chemical boundary species to be considered for the streams in the reacting system model.

Note that this step is not relevant in the case of flamelet import (Figure . : Defining Chemical Boundary

Species (p. )). For more information, see Defining the Stream Compositions (p. ).

Figure . : Defining Chemical Boundary Species

Steps in Using the Non-Premixed Model

. (steady diffusion flamelet model only) If you are generating flamelets, compute the flamelet state relation-

ships of species mass fractions, density, and temperature as a function of mixture fraction and scalar dis-

sipation (Figure . : Calculating Steady Diffusion Flamelets (p. )).

Figure . : Calculating Steady Diffusion Flamelets

. Compute the final chemistry look-up table, containing mean values of species fractions, density, and

temperature as a function of mean mixture fraction, mixture fraction variance, and possibly enthalpy and

scalar dissipation.The contents of this look-up table will reflect your preceding inputs describing the

turbulent reacting system (Figure . : Calculating the Chemistry Look-Up Table (p. )).

Figure . : Calculating the Chemistry Look-Up Table

The look-up table is the stored result of the integration of Equation . (or Equation .) and Equa-

tion . (in the Theory Guide). The look-up table will be used in ANSYS Fluent to determine mean

species mass fractions, density, and temperature from the values of mean mixture fraction ( ), mixture

fraction variance (

), and possibly mean enthalpy (

) and mean scalar dissipation (

) as they are

computed during the ANSYS Fluent calculation of the reacting flow. See Look-Up Tables for Adiabatic

Systems and Figure . : Visual Representation of a Look-Up Table for the Scalar (Mean Value of Mass

Fractions, Density, or Temperature) as a Function of Mean Mixture Fraction and Mixture Fraction Variance

in Adiabatic Single-Mixture-Fraction Systems and Figure . : Visual Representation of a Look-Up Table

for the Scalar as a Function of Mean Mixture Fraction and Mixture Fraction Variance and Normalized

Heat Loss/Gain in Non-Adiabatic Single-Mixture-Fraction Systems in the Theory Guide.

For a problem that includes a secondary stream (and, therefore, a second mixture fraction), you will

perform the first two steps listed above for the single-mixture-fraction approach and then prepare a

look-up table of instantaneous properties using Equation . or Equation . in the Theory Guide.

In the equilibrium chemistry model, the concentrations of species of interest are determined from the

mixture fraction using the assumption of chemical equilibrium (see Non-Premixed Combustion and

Mixture Fraction Theory in the Theory Guide). With this model, you can include the effects of interme-

diate species and dissociation reactions, producing more realistic predictions of flame temperatures

than the Eddy-Dissipation model. When you choose the equilibrium chemistry option, you will have

the opportunity to use the rich flammability limit (RFL) option.

To enable the equilibrium chemistry model

. Select Non-Premixed Combustion in the Species Model dialog box.

. Select Chemical Equilibrium in the Chemistry tab of the Species Model dialog box.

Setting Up the Equilibrium Chemistry Model

Figure . : The Species Model Dialog Box (Chemistry Tab)

... Choosing Adiabatic or Non-Adiabatic Options

... Specifying the Operating Pressure for the System

... Enabling a Secondary Inlet Stream

... Choosing to Define the Fuel Stream(s) Empirically

... Enabling the Rich Flammability Limit (RFL) Option

You should use the non-adiabatic modeling option if your problem definition in ANSYS Fluent will in-

clude one or more of the following:

radiation or wall heat transfer

multiple fuel inlets at different temperatures

multiple oxidant inlets at different temperatures

liquid fuel, coal particles, and/or heat transfer to inert particles

Note that the adiabatic model is a simpler model involving a two-dimensional look-up table in which

scalars depend only on  and

(or on

and

). If your model is defined as adiabatic, you will

not need to solve the energy equation in ANSYS Fluent and the system temperature will be determined

directly from the mixture fraction and the fuel and oxidant inlet temperatures. The non-adiabatic case

will be more complex and more time-consuming to compute, requiring the generation of three-dimen-

sional look-up tables. However, the non-adiabatic model option allows you to include the types of

reacting systems described above.

Select Adiabatic or Non-Adiabatic in the Chemistry tab of the Species Model dialog box.

The system Operating Pressure is used to calculate density using the ideal gas law. For non-adiabatic

simulations, the Compressibility Effects under PDF Options can be enabled to account for cases

where substantial pressure changes occur in time and/or space. In such cases it is assumed that the

species mass fractions do not change with pressure, and the density is calculated as

(.)

where

(.)

where

is the density at the specified Operating Pressure (

), and  is the local mean pressure

in an ANSYS Fluent cell.

When the Compressibility Effects option is enabled, the flow operating pressure (set in the Operating

Conditions dialog box) can differ from the Non-Premixed model operating pressure. To distinguish

this difference, the Operating Pressure name tag in the Species Model dialog box changes to Equi-

librium Operating Pressure when the compressibility effects option is enabled.

See Solution Strategies for Non-Premixed Modeling (p. ) for details about enabling compressibility

effects.

If you are modeling a system consisting of a single fuel and a single oxidizer stream, you do not need

to enable a secondary stream in your PDF calculation. As discussed in Definition of the Mixture Fraction

in the Theory Guide, a secondary stream should be enabled if your PDF reaction model will include

any of the following:

two dissimilar gaseous fuel streams

– In these simulations, the fuel stream defines one of the fuels and the secondary stream defines the second

fuel.

mixed fuel systems of dissimilar gaseous and liquid fuel

– In these simulations, the fuel stream defines the gaseous fuel and the secondary stream defines the liquid

fuel (or vice versa).

mixed fuel systems of dissimilar gaseous and coal fuels

– In these simulations, you can use the fuel stream or the secondary stream to define either the coal or

the gaseous fuel. See Modeling Coal Combustion Using the Non-Premixed Model (p. ) regarding coal

combustion simulations with the non-premixed combustion model.

mixed fuel systems of coal and liquid fuel

the liquid fuel. See Modeling Coal Combustion Using the Non-Premixed Model (p. ) regarding coal

coal combustion

– Coal combustion can be more accurately modeled by using a secondary stream to track the distinct

volatile and char off-gases.The fuel stream must define the char and the secondary stream must define

the volatile components of the coal. See Modeling Coal Combustion Using the Non-Premixed Model (p. )

regarding coal combustion simulations with the non-premixed combustion model.

a single fuel with two dissimilar oxidizer streams

– In these simulations, the fuel stream defines the fuel, the oxidizer stream defines one of the oxidizers,

and the secondary stream defines the second oxidizer.

To include a secondary stream in your model, turn on the Secondary Stream option under Stream

Options in the Chemistry tab.

Important

Using a secondary stream can substantially increase the calculation time for your simulation

since the multi-dimensional PDF integrations are performed at run time. Alternatively, ANSYS

Fluent can perform a full tabulation of the PDF integrations, as detailed in Full Tabulation

of the Two-Mixture-Fraction Model (p. ).

When the secondary stream is present, only instantaneous species mass fraction, temperature and

mixture properties are stored inside PDF table. The probability density function (PDF) calculates averaged

species mass fraction and mixture properties at the run time. After a PDF table has been generated

or read into ANSYS Fluent, you can select the shape of the assumed PDF from the Probability Density

Function drop-down list (PDF Options group box):

double delta: as given by Equation . in the Fluent Theory Guide.

beta: as given by Equation . in the Fluent Theory Guide.

The empirical fuel option provides an alternative method for defining the composition of the fuel or

secondary stream when the individual species components of the fuel are unknown. That is, you will

define the elemental fraction not the individual species. When this option is disabled, you will define

the chemical species that are present in each stream and the mass or mole fraction of each species,

as described in Defining the Stream Compositions (p. ). The option for defining an empirical fuel

stream is particularly useful for coal combustion simulations (see Modeling Coal Combustion Using

the Non-Premixed Model (p. )) or for simulations involving other complex hydrocarbon mixtures.

To define a fuel or secondary stream empirically

. Turn on the Empirical Fuel Stream option under Stream Options in the Chemistry tab of the Species

Model dialog box. If you have a secondary stream, enable the Empirical Secondary Stream option, or

both as appropriate.

. Specify the appropriate lower heating value (for example Empirical Fuel Lower Caloric Value, Empirical

Secondary Lower Caloric Value), specific heat (Empirical Fuel Specific Heat, Empirical Secondary

Specific Heat), and molecular weight (Empirical Fuel Molecular Weight, Empirical Secondary Molecular

Weight) for each empirically defined stream.

Important

The empirical definition option is available only with the full equilibrium chemistry model.

It cannot be used with the rich flammability limit (RFL) option or the steady and unsteady

diffusion flamelet models, since equilibrium calculations are required for the determination

of the fuel composition.

Important

The empirical fuel and secondary molecular weights are only required if your empirical

streams are entering the domain via an inlet boundary, or if you are using the partially

premixed model. If you are using the non-premixed model and the empirically defined

streams originate from the dispersed phase (for example, if you are modeling coal or liquid

fuel combustion) the molecular weights are not required for the computation.

You can define a rich limit on the mixture fraction when the equilibrium chemistry option is used. Input

of the rich limit is accomplished by specifying a value of the Rich Flammability Limit for the appro-

priate Fuel Stream, Secondary Stream, or both. You will not be allowed to specify the Rich Flammab-

ility Limit if you have used the empirical definition option for fuel composition.

ANSYS Fluent will compute the composition at the rich limit using equilibrium. For mixture fraction

values above this limit, ANSYS Fluent will suspend the equilibrium chemistry calculation and will

compute the composition based on mixing, but not burning, of the fuel with the composition at the

rich limit. A value of . for the rich limit implies that equilibrium calculations will be performed over

the full range of mixture fraction. When you use a rich limit that is less than ., equilibrium calculations

are suspended whenever ,

, or

exceeds the limit. This RFL model is often more accurate

than the assumption of chemical equilibrium for rich mixtures, and also avoids complex equilibrium

calculations, speeding up the preparation of the look-up tables. An RFL value of approximately twice

the stoichiometric mixture fraction is appropriate.

For the Secondary Stream, the rich flammability limit controls the equilibrium calculation for the

secondary mixture fraction. If your secondary stream is not a fuel, you should use an RFL value of .

A value of . for the rich limit implies that equilibrium calculations will be performed over the full

range of mixture fraction. When you input a rich limit that is less than ., equilibrium calculations are

suspended whenever

exceeds the limit. (Note that it is the secondary mixture fraction

and

not the partial fraction

that is used here.)

Important

Experimental studies and reviews [] (p. ), [] (p. ) have shown that although the

fuel-lean flame region approximates thermodynamic equilibrium, non-equilibrium kinetics

will prevail under fuel-rich conditions. Therefore, for non-empirically defined fuels, the RFL

model is strongly recommended.

To enable the diffusion flamelet models

. Select Steady Diffusion Flamelet or Unsteady Diffusion Flamelet in the Chemistry tab of the Species

Model dialog box. See Using the Unsteady Diffusion Flamelet Model (p. ).

Figure . : The Chemistry Tab for the Unsteady Diffusion Flamelet Model

... Specifying a Chemical Mechanism File for Flamelet Generation

... Importing a Flamelet

... Using the Unsteady Diffusion Flamelet Model

... Using the Diesel Unsteady Laminar Flamelet Model

... Resetting Diesel Unsteady Flamelets

Select Adiabatic or Non-Adiabatic in the Chemistry tab of the Species Model dialog box. See the

discussion in Choosing Adiabatic or Non-Adiabatic Options (p. ) about the two options.

The system Operating Pressure is used to calculate density using the ideal gas law. When the Com-

pressibility Effects option is enabled, the name Operating Pressure is changed to Equilibrium Op-

erating Pressure since the non-premixed combustion model operating pressure can differ from the

flow operating pressure. Specifying the Operating Pressure for the System (p. ) provides more in-

formation about this value.

You can use the steady or unsteady diffusion flamelet model for reactions in liquid systems. To do so,

enable Liquid Micro-Mixing under PDF Options. The Liquid Micro-Mixing option is discussed in

detail in Liquid Reactions in the Theory Guide.

If you are generating a flamelet file yourself, you will need to read in the chemical kinetic mechanism

and thermodynamic data. The mechanism and thermodynamic data must be in CHEMKIN format

[] (p. ).

To read in a CHEMKIN mechanism, select the Create Flamelet option in the Chemistry tab of the

Species Model dialog box and click the Import CHEMKIN Mechanism... button. Using the Import

CHEMKIN Format Mechanism dialog box, import the gas-phase files into ANSYS Fluent as described

in Importing a Volumetric Kinetic Mechanism in CHEMKIN Format (p. ). Note that for flamelet gen-

eration, only a gas-phase kinetic mechanism and a thermodynamic database are required.

Note that the import is limited to mechanisms with  or fewer species.

To import an existing flamelet file

. Select the Import Flamelet option in the Chemistry tab of the Species Model dialog box.

. (steady diffusion flamelet only) Select either Standard or CFX-RIF format under File Type.

. Click the Import Flamelet File... button. In The Select File Dialog Box (p. ), select the file (for a single

flamelet) or files (for multiple flamelets) to be read in to ANSYS Fluent.

After you have completed this step, you can skip ahead to the Table tab of the Species Model dialog

box (see Calculating the Look-Up Tables (p. )).

The unsteady diffusion flamelet model can only be enabled from a valid steady-state, steady diffusion

flamelet solution. When enabled, the unsteady diffusion flamelet model will change this case to unsteady

and postprocess marker probability equations on the frozen flow field. You should hence ensure that

the starting steady-state, steady diffusion flamelet solution is fully converged.

When the Unsteady Diffusion Flamelet is enabled in the Chemistry tab, the Import Flamelet File

for Restart... button appears in the dialog box, allowing you to run the simulation from a previously

saved case, data and unsteady flamelet file.

The Unsteady Diffusion Flamelet Model requires four user inputs in the Flamelet tab:

The Number of Grid Points in Flamelet.

The Mixture Fraction Lower Limit for Initial Probability.The initial condition of the marker probability

field is unity for all mean mixture fractions above the Mixture Fraction Lower Limit for Initial Probability,

and zero for mean mixture fractions below it. Note that this should be specified to be greater than the

stoichiometric mixture fraction.

Setting Up the Steady and Unsteady Diffusion Flamelet Models

Maximum Scalar Dissipation. Flamelets may extinguish at high scalar dissipations because diffusion in

the flamelet overwhelms reaction. It is possible to have unrealistically high modeled scalar dissipation in

the 2D or 3D ANSYS Fluent simulations, which gets transferred to the 1D unsteady flamelet. In order to

avoid excessive diffusion in the 1D unsteady flamelet, the instantaneous scalar dissipation in the 1D

flamelet is limited to the specified Maximum Scalar Dissipation.

Courant Number.The time step for the unsteady probability marker equation is calculated automatically

by ANSYS Fluent based on the Courant Number. Larger values imply fewer time steps to convect/diffuse

the marker probability out of the domain, but also results in a larger numerical error.The Courant Number

should be small enough so that the unsteady flamelet mean mass fractions are unchanged with any

smaller Courant Number.The default value of  should be sufficient for most applications.

Number of Flamelets.The number of unsteady laminar flamelets that ANSYS Fluent will generate during

the run.The marker probability equation Equation . in the Fluent Theory Guide will be solved for each

flamelet.

When these inputs have been set, clicking the Initialize Unsteady Flamelet Probability button initial-

izes the marker probability equation for each flamelet, automatically enabling the Unsteady solver,

while disabling all equations except the Unsteady Flamelet Probability equation in the Solution

Controls task page. This initialization in the Flamelet tab also sets the Time Step Size in the Run

Calculation task page.

Important

Do not initialize your solution from the tree or the Solution Initialization task page. Note that

you are postprocessing a probability field on the frozen steady-state flow field, and by clicking

the Initialize Unsteady Flamelet Probability button, you have already initialized the probab-

ility marker field.

If you disable the Unsteady Diffusion Flamelet model and you want to revert to solving a

steady diffusion flamelet simulation, make sure you enable Steady (either in the General task

page or in the tree from the Setup/General/ Analysis Type tree item) and enable all the

equations (in the Solution Controls task page or in the tree from the Solution/Solution Controls

tree item).

The diesel unsteady laminar flamelet model can only be enabled when conditions for compression-

ignition are met:

The Transient solver is selected in the General task page (or in the tree from the Setup/General/ Analysis

Type).

The In-Cylinder dynamic mesh is enabled.

The Discrete Phase model option Interaction with Continuous Phase is selected.

The basic steps for setting the diesel unsteady laminar flamelet models are as follows.

. In the Chemistry tab, select Diesel Unsteady Flamelet.

Figure . : The Enabled Diesel Unsteady Flamelet Model

. If a detailed chemical mechanism containing kinetic reactions appropriate for compression ignition has

not yet been defined in your case, you can import a mechanism in CHEMKIN format as described in Im-

porting a Volumetric Kinetic Mechanism in CHEMKIN Format (p. ).

The mechanism can include pollutant formation reactions as well if you are interested in modeling

emissions.

. In the Boundary tab, define the stream compositions as described in Defining the Stream Composi-

. In the Flamelet tab, set the following flamelet parameters.

a.

Set the Number of Grid Points in Flamelet.

b. Set the Number of Unsteady Flamelets that ANSYS Fluent will generate during simulation.

c.

a.

c.

(for multiple unsteady flamelets) Set the flamelet start times.

ANSYS Fluent automatically sets the start time for the first flamelet, but you must set the start

time for each consecutive flamelet using the Unsteady Flamelet Parameters dialog box. Open

it by clicking Set Flamelet Parameters and enter the start time for each flamelet either in

seconds or in crank angles if the dynamic mesh is enabled.

Figure . : The Unsteady Flamelet Parameters Dialog Box

ANSYS Fluent starts simulation with only one flamelet, and then it automatically introduces

new flamelets into the reacting domain at the times you have specified.

d. The default initial condition for an unsteady flamelet is unburnt. ANSYS Fluent provides the Burnt

Initial Flamelet option that allows you to set the initial flamelet condition to a chemical equilibrium

burnt state.This option is useful if you are modeling internal combustion engines where residual gases

may be present in the cylinder before the spray is injected, which would be incorrectly modeled by

the unburnt state. Note that the Burnt Initial Flamelet is only used at case initialization.

e. (optional) Specify the flamelet fluid zones.

ANSYS Fluent calculates diesel unsteady flamelets using the zone-averaged pressure and scalar

dissipation at every time step. By default, the averaging is performed over all fluid zones in the

domain, but you can also select and/or deselect the fluid zones using the Flamelet Fluid Zones

dialog box. Open this dialog box by clicking Set Flamelet Fluid Zones and select the fluid

zones to be used for calculating average pressure and scalar dissipation. If no fluid zone is se-

lected, ANSYS Fluent will compute domain average pressure and scalar dissipation using all

fluid zones.

Figure . : The Flamelet Fluid Zones Dialog Box

Note

For internal combustion cases, it is recommended that you select the cylinder fluid

zones and deselect the intake and exhaust fluid zones.

Note that ANSYS Fluent calculates flamelets at every time step of the  run. For this reason, the option

to calculate the flamelets as a preprocessing step before running your simulation is unavailable,

and Calculate Flamelets appears dimmed.

. In the Table tab, set the PDF table parameters as described in Calculating the Look-Up Tables (p. ).

Note that ANSYS Fluent calculates PDF table at every time step of the  run. For this reason, the

option to calculate the PDF table as a preprocessing step before running your simulation is unavail-

able, and Calculate PDF Table appears dimmed.

.... Recommended Settings for Internal Combustion Engines

When setting up and using the Diesel Unsteady Flamelet model for internal combustion engine sim-

ulations, the following recommendations apply:

. Number of Flamelets

a.

You must specify at least two diesel unsteady flamelets. ANSYS Fluent will use the first flamelet to

model trapped burnt gases from the previous cycle.The second flamelet will start at the crank angle

(CA) of fuel injection, specified in the Unsteady Flamelet Parameters dialog box (see Figure . :The

Flamelet Fluid Zones Dialog Box (p. )).

b. To model split injections where an initial fuel mass is injected and burns before the main fuel injection,

three or more unsteady flamelets are required.

. Flamelet Initialization

By default, the flamelet is initialized as mixed-but-unburnt. However, in all practical scenarios there

is always some trapped gas remaining inside the cylinder. Therefore, it is recommended that you

use the Burnt Initial Flamelet option in the Unsteady Flamelet Parameters dialog box (see

Figure . : The Flamelet Fluid Zones Dialog Box (p. )). When this option is selected, ANSYS

Fluent performs a constant temperature equilibrium calculation and sets the initial flamelet con-

dition to a chemical equilibrium burnt state.

. Multi-cycle simulations

a.

To accurately model multiple cycles of internal combustion engines, the flamelets must be reset at

the end of each cycle.This is performed by defining the Diesel Unsteady Flamelet Reset event,

typically at the specified crank angle, just before the inlet valve opens. Refer to the Resetting Diesel

Unsteady Flamelets (p. ) for details.This approach is recommended for modeling the EGR trapped

gases with the first burnt unsteady flamelet.

b. If you are using the Inert (EGR) model in order to track the trapped inert mixture, you need to define

the Inert EGR Reset event at the specified crank angle just before the inlet valve opens. See Resetting

Inert EGR (p. ) for details.

In order to simulate multiple cycles in internal combustion engines, flamelets should be reset at the

end of every cycle. In addition, the burned trapped gases must be modeled, which can be done in

one of the two ways. The first and recommended approach is to use the Diesel Unsteady Flamelet

Reset option. The second approach is to use the inert (EGR) model and the Inert EGR Reset option.

You can access the Diesel Unsteady Flamelet Reset and Inert EGR Reset options via the Dynamic

Mesh Events dialog box. There, you need to set the crank angle at which this event occurs (usually

shortly before the inlet valves open) and the participating fluid zones (usually only the combustion

chamber and not the intake and exhaust port zones).

When the Diesel Unsteady Flamelet Reset event is executed, all flamelets are deleted and a new

flamelet is introduced with a state set to the probability-weighted average condition of all flamelets

present before reset. The other new flamelets are introduced during a new cycle in a similar fashion

to that described in Using the Diesel Unsteady Laminar Flamelet Model (p. ).

When the inert EGR reset event is executed with the diesel unsteady flamelet model, the burnt gas in

the selected Inert EGR Reset zones is converted to inert, all flamelets are deleted, and a new unburnt

flamelet is introduced into the domain.

Note

The Diesel Unsteady Flamelet Reset option is available only when the selected number

of flamelets is greater than one.

In modeling a non-premixed combustion problem, you will only specify the boundary species (that is,

the fuel, oxidizer, and if necessary, secondary stream species). The intermediate and product species

will be determined automatically.

ANSYS Fluent provides you with an initial list of common boundary species (ch4, h2, jet-a<g>, n2

and o2). If your fuel and/or oxidizer is composed of different species, you can add them to the

boundary Species list. All boundary species must exist in the chemical database and you must enter

their names in the same format used in the database, otherwise an error message will be issued.

After defining the boundary species that will be considered in the reaction system, you must define

their mole or mass fractions at the fuel and oxidizer inlets and at the secondary inlet, if one exists. (If

you choose to define the fuel or secondary stream composition empirically, you will instead enter the

parameters described at the end of this section.) For the example shown in Figure . : Chemical Systems

That Can Be Modeled Using a Single Mixture Fraction in the Theory Guide, for example, the fuel inlet

consists of % CO4, % CO, % CO2, and % C3H8.

Finally, the inlet stream temperatures of your reacting system are required for construction of the look-

up table and computation of the equilibrium chemistry model.

For the equilibrium chemistry model, the species names are entered using the Boundary tab in the

Species Model dialog box (Figure . : The Species Model Dialog Box (Boundary Tab) (p. )). If you

are generating a steady or unsteady diffusion flamelet, the list of boundary species will be automatically

filled as all the species in the CHEMKIN mechanism, and you will be unable to change these.

Figure . : The Species Model Dialog Box (Boundary Tab)

The steps for adding new species and defining their compositions are as follows:

. (chemistry equilibrium chemistry model only) If your fuel, oxidizer, or secondary streams are composed of

species other than the default species list, type the chemical formula (for example, so2 or SO2 for SO )

under Boundary Species and click Add.The species will be added to the Species list. Continue in this

manner until all of the boundary species you want to include are shown in the Species list.

To remove a species from the list, type the chemical formula under Boundary Species and click

Remove. To print a list of all species in the thermodynamic database file (thermo.db) in the console

window, click List Available Species.

. (non-equilibrium chemistry models) Optionally, select the boundary species as described in Overview of

the Problem Setup Procedure (p. ).

. Under Specify Species In, specify whether you want to enter the Mass Fraction or Mole Fraction. Mass

Fraction is the default.

Defining the Stream Compositions

. For each relevant species in the Species list, specify its mass or mole fraction for each stream (Fuel, Oxid,

or Second as appropriate) by entering values in the table. Note that if you change from Mass Fraction to

Mole Fraction (or vice versa), all values will be automatically converted if they sum to  or , so be sure

that you are entering either all mass fractions or all mole fractions as appropriate. If the values do not sum

to  or , an error will be issued.

. Under Temperature, specify the following inputs:

Fuel

is the temperature of the fuel inlet in your model. In adiabatic simulations, this input (together with

the oxidizer inlet temperature) determines the inlet stream temperatures that will be used by ANSYS

Fluent. In non-adiabatic systems, this input should match the inlet thermal boundary condition that

you will use in ANSYS Fluent (although you will enter this boundary condition again in the ANSYS Fluent

session). If your ANSYS Fluent model will use liquid fuel or coal combustion, define the inlet fuel tem-

perature as the temperature at which vaporization/devolatilization begins (that is, the Vaporization

Temperature specified for the discrete-phase material—see Setting Material Properties for the Discrete

Phase (p. )). For such non-adiabatic systems, the inlet temperature will be used only to adjust the

look-up table grid (for example, the discrete enthalpy values for which the look-up table is computed).

Note that if you have more than one fuel inlet, and these inlets are not at the same temperature, you

must define your system as non-adiabatic. In this case, you should enter the fuel inlet temperature as

the value at the dominant fuel inlet.

Oxid

is the temperature of the oxidizer inlet in your model.The issues raised in the discussion of the input

of the fuel inlet temperature (directly above) pertain to this input as well.

Second

is the temperature of the secondary stream inlet in your model. (This item will appear only when you

have defined a secondary inlet.) The issues raised in the discussion of the input of the fuel inlet temper-

ature (directly above) pertain to this input as well.

... Setting Boundary Stream Species

... Modifying the Database

... Composition Inputs for Empirically-Defined Fuel Streams

... Modeling Liquid Fuel Combustion Using the Non-Premixed Model

... Modeling Coal Combustion Using the Non-Premixed Model

In combustion, a large number of intermediate and product species may be produced from a small

number of initial boundary species. In ANSYS Fluent you must specify only the species composition of

your boundary species in the fuel, oxidizer, and (if appropriate) secondary streams. ANSYS Fluent will

calculate all intermediate and product species automatically. The following suggestions may be helpful

in the definition of the system chemistry:

For coal combustion, char in the coal should be represented by C(s).

Important

Care should be taken to distinguish atomic carbon, C, from solid carbon, C(s). Atomic

carbon should be selected only if you are using the empirically-defined input method.

If your fuel composition is known empirically (for example, C0. H3 O0. ), use the option for an empirically-

defined stream (see below).

If you want to include the sulfur that may be present in a hydrocarbon fuel, note that this may hinder the

convergence of the equilibrium solver, especially if the concentration of sulfur is small. It is therefore re-

commended that you include sulfur in the calculation only if it is present in considerable quantities.

.... Including Condensed Species

In addition to gaseous species, liquid and solid species can be included in the chemistry calculations.

They are often indicated by an “l” or an “s” in parentheses after the species name. If you add a con-

densed species to the equilibrium chemical system, its density will be retrieved from ANSYS Fluent’s

chemical property database file propdb.scm if you are using the thermodynamic database file

thermo.db that is also supplied with ANSYS Fluent. If you are using a custom thermodynamic

database file and want to include a condensed species in the equilibrium system that does not exist

in propdb.scm, a density of  kg/m3 will be assumed. The condensed species density can be

changed in the Create/Edit Materials Dialog Box (p. ) after the PDF table has been calculated. If

you modify the condensed species density in this manner, you will then need to recalculate the PDF

table.

If you want to include a new species in your reacting system that is not available in the chemical

database, you can add it to the database file, thermo.db. The format for thermo.db is detailed in

[] (p. ). If you choose to modify the standard database file, you should create copies of the original

file.

As mentioned in Defining the Problem Type (p. ), you can define the composition of a fuel stream

(that is, the standard fuel or a secondary fuel) empirically. For an empirically-defined stream, you will

need to enter the atomic mass or mole fractions in addition to the inputs for lower caloric (heating)

value of the fuel and the mean specific heat of the fuel that were described previously.

The heat of formation of an empirically defined stream is calculated from the heating value and the

atomic composition. The fuel inlet temperature and fuel specific heat are used to calculate the sensible

enthalpy. The molecular weight is used for the computation of the unburnt stream density. Note that

the unburnt density is only required if the stream enters via an inlet boundary, or if you are using the

partially-premixed model.

When an empirically-defined fuel or secondary stream is specified in the Chemistry tab (equilibrium

chemistry model only) of the Species Model dialog box, you must specify the atom fractions of C, H,

O, N, and S in that stream instead of the species mass or mole fractions. To avoid confusion, the species

fraction inputs for an empirically-defined stream will be grayed out in the table within the Boundary

tab, leaving only the fields for atom fractions (that is, c, h, o, n, and s).

Liquid fuel combustion can be modeled with the discrete phase and non-premixed models. In ANSYS

Fluent, the fuel vapor, which is produced by evaporation of the liquid fuel, is defined as the fuel stream.

(See Defining the Stream Compositions (p. ).) The liquid fuel that evaporates within the domain

appears as a source of the mean fuel mixture fraction.

Within ANSYS Fluent, you define the liquid fuel discrete-phase model in the usual way. The gas phase

(oxidizer) flow inlet is modeled using an inlet mixture fraction of zero and the fuel droplets are intro-

duced as discrete phase injections (see Setting Initial Conditions for the Discrete Phase (p. )). The

property inputs for the liquid fuel droplets are unaltered by the non-premixed model (see Setting

Material Properties for the Discrete Phase (p. )). Note that when you are requested to input the gas

phase species destination for the evaporating liquid, you should specify the species that make up the

evaporating stream.

If the fuel stream was defined as a mixture of components, you should select the largest of these

components as the “evaporating species”. ANSYS Fluent will ensure that the mass evaporated from

the liquid droplet enters the gas phase as a source of the fuel mixture that you defined. The evaporating

species you select here is used only to compute the diffusion controlled driving force in the evaporation

rate.

If your model involves coal combustion, the fuel and secondary stream compositions can be input in

one of several ways. You can use a single mixture fraction (fuel stream) to represent the coal, defining

the fuel composition as a mixture of volatiles and char (solid carbon). Alternatively, you can use two

mixture fractions (fuel and secondary streams), defining the volatiles and char separately. In two-mixture-

fraction models for coal combustion, the fuel stream represents the char and the secondary stream

represents volatiles. This section describes the modeling options and special input procedures for coal

combustion models using the non-premixed approach.

There are three options for coal combustion:

When coal is the only fuel in the system, you can model the coal using two mixture fractions, where the

primary stream represents the char and the secondary stream represents the volatiles. Generally, the char

stream composition is defined as % C(s).The volatile stream composition is defined by selecting appro-

priate species and setting their mole or mass fractions. Alternatively, you can use the empirical method

(input of atom fractions) for defining these compositions.

Important

Using two mixture fractions to model coal combustion is more accurate than using one

mixture fraction as the volatile and char streams are modeled separately. However, the

two-mixture-fraction model incurs significant additional computational expense since the

multi-dimensional PDF integrations are performed at run time.

When coal is the only fuel in the system, you can choose to model the coal using a single mixture fraction

(the fuel stream).When this approach is adopted, the fuel composition you define includes both volatile

species and char. Char is typically represented by including C(s) in the species list.You can define the fuel

stream composition by selecting appropriate species and setting their mole fractions, or by using the em-

pirical method (input of atom fractions). Definition of the composition is described in detail below.

Important

Using a single mixture fraction for coal combustion is less accurate than using two mixture

fractions. However, convergence in ANSYS Fluent should be substantially faster than the

two-mixture-fraction model.

When coal is used with another (gaseous or liquid) fuel of different composition, you must model the coal

with one mixture fraction and use a second mixture fraction to represent the second (gaseous or liquid)

fuel.The stream associated with the coal composition is defined as detailed below for single-mixture-

fraction models.

.... Defining the Coal Composition: Single-Mixture-Fraction Models

When coal is modeled using a single mixture fraction (the fuel stream), the fuel stream composition

can be input using the conventional approach or the empirical fuel approach.

Conventional approach:

To use the conventional approach, you will need to define the mixture of species in the coal and

their mole or mass fractions in the fuel stream. Use the Boundary tab in the Species Model dialog

box to input the list of species (for example, C3H8, CH4, CO, CO2, C(s)) that approximate the coal

composition, and their mole or mass fractions.

Note that C(s) is used to represent the char content of the coal. For example, consider a coal that

has a molar composition of % volatiles and % char on a dry ash free (DAF) basis. Assuming

the volatiles can be represented by an equimolar mixture of C3H8 and CO, the fuel stream compos-

ition defined in the Boundary tab would be C3H8=., CO = ., and C(s)=.. Note that the coal

composition should always be defined on an ash-free basis, even if ash will be considered in the

ANSYS Fluent calculation.

To define ash properties, go to the Create/Edit Materials dialog box and select combusting-

particle as the Material Type.

The following table illustrates the conversion from a typical mass-based proximate analysis to the

species fraction inputs required by ANSYS Fluent. Note that the conversion requires that you make

an assumption regarding the species representing the volatiles. Here, the volatiles are assumed to

exist as an equimolar mix of propane and carbon monoxide.

Mole Fraction

(DAF)

Moles (DAF)

Mass Fraction

(DAF)

Weight %

Proximate Analysis

Volatiles

.

.

.

–C3H8

.

.

.

– CO

.

.

.

Fixed Carbon (C(s))

Ash

.

.

(Total)

Moisture in the coal can be considered by adding it in the fuel composition as liquid water, H2O(l).

The moisture can also be defined as water vapor, H2O, provided that the corresponding latent heat

is included in the discrete phase material inputs in ANSYS Fluent. If the liquid water is used as a

boundary species, it should be removed from the list of excluded species (see Forcing the Exclusion

and Inclusion of Equilibrium Species (p. )).

Important

Note that if water is included in the coal, the water release is not modeled as evaporation,

which is typically the case in the wet combustion model, described in Particle

Types (p. ).

Empirical fuel approach:

To use the empirical approach, enable the Empirical Fuel Stream option in the Chemistry tab.

This method is ideal if you have an elemental analysis of the coal.

In the Chemistry tab, enter the lower heating value and mean specific heat of the coal. ANSYS

Fluent will use these inputs to determine the mole fractions of the chemical species you have in-

cluded in the system. Then, in the Boundary tab, define the atom fractions of C, H, N, S, and O in

the fuel stream.

Note that for both of these composition input methods, you should take care to distinguish atomic

carbon, C, from solid carbon, C(s). Atomic carbon should only be selected if you are using the empir-

ical fuel input method.

See Additional Coal Modeling Inputs in ANSYS Fluent (p. ) for details about further inputs for

modeling coal combustion.

.... Defining the Coal Composition: Two-Mixture-Fraction Models

You can model coal using the two mixture fractions model, where the primary stream represents the

char and the secondary stream represents the volatiles.

As in single-mixture-fraction cases, the fuel stream and secondary stream compositions in a two-

mixture-fraction case can be entered using either the conventional approach or the empirical fuel

approach.

their mole or mass fractions in the fuel and secondary streams.

Use the Boundary tab of Species Model dialog box to define the mole or mass fractions of volatile

species in the secondary stream (for example, C3H8, CH4, CO, CO2, C(s)). Next, define the mole or

mass fractions of species used to represent the char. Generally, you will specify % C(s) for the

fuel stream.

To use the empirical fuel approach, enable the Empirical Secondary Stream option in the Chemistry

tab for the volatile (secondary) stream. This method is ideal if you have an elemental analysis of

the coal.

In the Chemistry tab, input the lower heating value and mean specific heat of the coal volatiles.

the coal.

Then, in the Boundary tab, define the mole or mass fractions of species used to represent the char.

Generally, you will specify % C(s) for the fuel stream. Finally, define the atom fractions of C, H,

N, S, and O in the volatiles. ANSYS Fluent will use these inputs to determine the mole fractions of

the chemical species you have included in the system. For example, consider coal with the following

DAF (dry ash free) data and elemental analysis:

Wt % (DAF)

Wt % (dry)

.

Volatiles

.

Char (C(s))

Ash

Wt % (DAF)

Wt % (DAF)

Element

.

.

C

.

.

H

.

.

O

.

.

N

.

S

(Note that in the final column, for modeling simplicity, the sulfur content of the coal has been

combined into the nitrogen mass fraction.)

You can combine the proximate and ultimate analysis data to yield the following elemental com-

position of the volatile stream:

Moles

Mass

Element

.

.

.

(. - .)

C

.

.

.

H

.

.

.

.

O

.

.

.

.

N

.

.

Total

This adjusted composition is used to define the secondary stream (volatile) composition.

The lower heating value of the volatiles can be computed from the known heating value of the

coal and the char (DAF):

You can compute the heating value of the volatiles as

(.)

or

(.)

.... Additional Coal Modeling Inputs in ANSYS Fluent

Within ANSYS Fluent, the DPM coal combustion simulation is defined as usual when the non-premixed

combustion model is selected. The air (oxidizer) inlets are defined as having a mixture fraction value

of zero. No gas phase fuel inlets will be included and the sole source of fuel will come from the coal

devolatilization and char burnout. The coal particles are defined as injections using the Set Injection

Properties dialog box in the usual way, and physical properties for the coal material are specified as

described in Setting Material Properties for the Discrete Phase (p. ). Remember the following issues

when you are defining injections and discrete-phase material properties for coal materials:

In the Set Injection Properties dialog box, you will specify for the Oxidizing Species one of the compon-

ents of the oxidizer stream.This species concentration field will be used to calculate the diffusion-controlled

driving force in the char burnout law (if applicable), and is O2 by default.

The specification of the char and volatile streams differs depending on the type of model you are

defining:

– If coal is modeled using a single mixture fraction, the gas phase species representing the volatiles and

the char combustion are represented by the mixture fraction used by the non-premixed combustion

model.

– If coal is modeled using two mixture fractions, rather than specifying a destination species for the

volatiles and char, you will instead specify the Devolatilizing Stream (as secondary) and the Char

Stream (as primary).

– If coal is modeled using one mixture fraction, and another fuel is modeled using a second mixture

fraction, you should specify the stream representing the coal as both the Devolatilizing Stream and

the Char Stream.

In the Create/Edit Materials dialog box, Vaporization Temperature should be set equal to the fuel inlet

temperature.This temperature controls the onset of the devolatilization process.The fuel inlet temperature

that you define in the Boundary tab of the Species Model dialog box should be set to the temperature

at which you want to initiate devolatilization.This way, the look-up tables will include the appropriate

temperature range for your process.

In the Create/Edit Materials dialog box, Volatile Component Fraction and Combustible Fraction should

be set to values that are consistent with the coal composition used to define the fuel (and secondary)

stream composition.

Also in the Create/Edit Materials dialog box, you will be prompted for the Burnout Stoichiometric Ratio

and for the Latent Heat.The Burnout Stoichiometric Ratio is used in the calculation of the diffusion

controlled burnout rate but has no other impact on the system chemistry when the non-premixed com-

bustion model is used.The Burnout Stoichiometric Ratio is the mass of oxidant required per mass of

char.The default value of . assumes that C(s) is oxidized by O2 to yield CO2.The Latent Heat input

determines the heat required to generate the vapor phase volatiles defined in the non-premixed system

chemistry.You can usually set this value to zero when the non-premixed model is used, since your

definition of volatile species will have been based on the overall heating value of the coal. However, if

the coal composition includes the water content, the latent heat should be set as follows:

– Set the latent heat to zero if the water content of the coal has been defined as H2O(L). In this case, the

system chemistry will include the latent heat required to vaporize the liquid water.

– Set the latent heat to the value for water (. J/kg), adjusted by the mass loading of water in

the volatiles, if the water content of the coal has been defined using water vapor, H2O. In this case, the

water content you defined will be evolved along with the other species in the coal but the system

chemistry does not include the latent heat effect.

The Density you define for the coal in the Create/Edit Materials dialog box should be the apparent

density, including ash content.

You will not be asked to define the Heat of Reaction for Burnout for the char combustion.

.... Postprocessing Non-Premixed Models of Coal Combustion

ANSYS Fluent reports the rate of volatile release from the coal using the DPM Evaporation/Devolat-

ilization postprocessing variable. The rate of char burnout is reported in the DPM Burnout variable.

....The Coal Calculator

The Coal Calculator dialog box automates the calculations described above for setting up a coal

case from the proximate and ultimate analyses.

The inputs to the Coal Calculator dialog box are:

. Coal Proximate Analysis, which is the mass fraction of Volatile, Fixed Carbon, Ash and Moisture in

the coal.

the coal.

Free (DAF) coal.

. The option to use a Secondary Stream. If enabled, the two mixture fraction model will be set with the

primary stream representing char as

, and an empirical secondary stream representing the volatiles.

. The Coal Particle Material Name. A DPM Combusting Particle Material will be created with this name.

. The Coal As-Received HCV (Higher Calorific Value).

. The High Temperature Volatile Yield. Proximate analyses are generally done with slower heating rates

and lower temperatures than would occur in a real flame.Therefore, enhanced devolatization at higher

temperatures can cause the volatile yield to exceed the proximate analysis fraction.To model this, the

actual volatile fraction used is calculated as that specified in the Proximate Analysis input multiplied

by the High Temperature Volatile Yield.The actual Fixed Carbon fraction is then calculated as one

minus the sum of the actual Volatile, Ash, and Moisture fractions.

NOx model.

When the OK button is clicked, ANSYS Fluent makes the following changes:

a.

The empirical fuel atomic compositions in the Boundary tab are set, and the Non-Adiabatic model

is enabled as required for DPM.The Empirical Fuel Lower Calorific Value is calculated as follows. First

the DAF LCV of the coal is computed as,

(.)

where

and

(.)

where

and

are the proximate moisture and ash fractions,

is the ultimate

fraction,

and

are the molecular weight of water and atomic hydrogen, respectively,

and

is the latent heat of water.

If you are using the Secondary Stream option,

using,

(.)

where

and

are the proximate fixed carbon and volatile fractions, respect-

ively.

b. A combusting particle material is created with Volatile Component Fraction and Combustible

Fraction calculated from the ultimate and proximate analyses.The Discrete Phase Model (DPM) is

enabled.

c.

For the Fuel NOx model, the char N conversion is set to NO, and the Fuel NOx  Volatile and Char

mass fractions are set according to the ultimate and proximate compositions. Note that even though

some of the Fuel NOx parameters are changed, the Fuel NOx model itself is not enabled.

After the Coal Calculator has set up the relevant models, you must build the PDF Table by clicking

Calculate PDF Table in the Table tab. You will also need to create injections if you have not done

this yet. After converging your coal combustion case, you may want to enable the NOx model for

postprocessing nitrogen-oxide pollutants.

For information about setting up control parameters, see the following sections:

... Forcing the Exclusion and Inclusion of Equilibrium Species

... Defining the Flamelet Controls

... Zeroing Species in the Initial Unsteady Flamelet

Setting Up Control Parameters

Because ANSYS Fluent calculates all intermediate and product species automatically during the equi-

librium calculation, certain species will be included that are generally not in chemical equilibrium.

Principal among these are the NOx species. Specifically, the NOx reaction rates are slow and should

not be treated using an equilibrium assumption. Instead, the NOx concentration is predicted most

accurately using the ANSYS Fluent NOx postprocessor, where finite-rate kinetics are included (see

NOx Formation (p. )). The NOx species can be safely excluded from the equilibrium calculation since

they are present at low concentrations and have little impact on the density, temperature, and other

species.

To force the exclusion of a species from the equilibrium calculation, click the Control tab in the Species

Model dialog box (Figure . : The Species Model Dialog Box (Control Tab) (p. )).

Figure . : The Species Model Dialog Box (Control Tab)

Under Species Excluded From Equilibrium, enter the chemical formula for the desired species in the

Add/Remove Species field. Next, click Add to add the species to the Species list or Remove to remove

an existing species from the Species list.

If there are species that you want to include in your PDF table that would be ignored by ANSYS Flu-

ent due to their low concentration (for example, CH, CH2, CH3 for the NOx calculation), you can force

ANSYS Fluent to include them using the text interface:

define → models → species → non-premixed-combustion

When the console window prompts you with Force Equilibrium Species to Include...,

specify the appropriate species by entering the chemical formula(s) in double quotes (for example,

"ch", "ch2").

Note that you will have to first set up the inputs for the fuel and oxidizer before you are given the

option to include the species.

When the steady diffusion flamelet model is selected, and you have created or imported a flamelet,

you can adjust the controls for the flamelet solution in the Control tab of the Species Model dialog

box (Figure . : The Species Model Dialog Box (Control Tab) for the Steady Diffusion Flamelet Mod-

el (p. )).

Figure . : The Species Model Dialog Box (Control Tab) for the Steady Diffusion Flamelet

Model

The Initial Fourier Number sets the first time step for the solution of the flamelet equations (Equa-

tion . and Equation . in the Theory Guide). This first time step is calculated as the explicit stability-

limited diffusion time step multiplied by this value. If the solution diverges before the first time step

is complete, the value should be lowered.

The Fourier Number Multiplier increases the time step at subsequent times. Every time step after

the first is multiplied by this value. If the solution diverges after the first time step, this value should

be reduced.

During the numerical integration of the flamelet equations, the local error is controlled to be less than

(.)

where

represents the species mass fractions and temperature at point  in the 1D flamelet.

is

the value of the Relative Error Tolerance and

(.)

where

is

is the value of the Absolute Error Tolerance, both

of which you can specify.

Because steady flamelets are obtained by time-stepping, they are considered converged only when

the maximum absolute change in species fraction or temperature at any discrete mixture-fraction point

is less than the specified Flamelet Convergence Tolerance. Between time steps, the flamelet species

fractions and temperature will sometimes oscillate, which causes absolute changes that are always

greater than the flamelet convergence tolerance. In such cases, ANSYS Fluent will stop the flamelet

calculation after the total elapsed time has exceeded the Maximum Integration Time.

When modeling gas-phase combustion using the Eulerian unsteady laminar flamelet model, the

flamelet fields are initialized to a burning, steady-flamelet solution in order to model ignition. However,

assuming steady-flamelet profiles for slow-forming species is inaccurate. A better approximation is to

identify the slow species and to set them to zero, which is done in the Control tab. By default, ANSYS

Fluent selects some NOx species (NO, NO2, N2O, N, NH, NH2, NH3, NNH, HCN, HNO, CN, H2CN, HCNN,

HCNO, HOCN, HNCO, HCO), as well as liquid water H2<l> and solid carbon C<s> to be zeroed. See

Figure . : Method to Zero Out the Slow Chemistry Species (p. ).

Figure . : Method to Zero Out the Slow Chemistry Species

For information about calculating flamelets, see the following sections:

... Steady Diffusion Flamelet

... Unsteady Diffusion Flamelet

... Saving the Flamelet Data

... Postprocessing the Flamelet Data

In the Flamelet tab of the Species Model dialog box (Figure . : The Species Model Dialog Box

(Flamelet Tab) (p. )), you will enter values for parameters of the flamelet(s).

Figure . : The Species Model Dialog Box (Flamelet Tab)

The Flamelet Parameters are as follows:

Number of Grid Points in Flamelet

specifies the number of mixture fraction grid points distributed between the oxidizer (

) and the fuel

(

). Increased resolution will provide greater accuracy, but since the flamelet species and temperature

are solved coupled and implicit in  space, the solution time and memory requirements increase greatly

with the number of  grid points.

Maximum Number of Flamelets

specifies the maximum number of flamelet profiles to be calculated. If the flamelet extinguishes before

this number is reached, flamelet generation is halted and the actual number of flamelets in the flamelet

library will be less than this value.

Initial Scalar Dissipation

is the scalar dissipation of the first flamelet in the library.This corresponds to

Scalar Dissipation Multiplier

specifies the ratio of the scalar dissipation step in which successive flamelets are generated when the

scalar dissipation is less than  s-.This corresponds to

for <  in Equation . in the Theory Guide.

Calculating the Flamelets

Scalar Dissipation Step

specifies the interval between scalar dissipation values (in s-) for which multiple flamelets will be calculated.

This corresponds to

for ≥  in Equation . in the Theory Guide.

Note

Scalar Dissipation Multiplier and Scalar Dissipation Step are used to specify the in-

terval of scalar dissipation for <  and ≥ , respectively. For example, for initial scalar

dissipation of 1e- s- with a Scalar Dissipation Multiplier of , and a Scalar Dissipa-

tion Step of , the flamelets will be generated with scalar dissipations of 1e-, 1e-, .,

., , , , and so on.

User Defined Flamelet Parameters

enables you to hook a user-defined function for scalar dissipation and mean mixture fraction (or progress

variable) grid discretization

Automated Grid Refinement

employs an adaptive algorithm, which inserts grid points so that the change of values, as well as the

change of slopes, between successive grid points is less than user-specified tolerances. For information

about this option, refer to Steady Diffusion Flamelet Automated Grid Refinement in the Theory Guide.

Once this option is enabled, you can specify the following parameters:

Initial Number of Grid Points in Flamelet

calculates a steady solution on a coarse grid, with a default of . See Equation . in the Theory

Guide.

Maximum Number of Grid Points in Flamelet

has a default of

.

Maximum Change in Value Ratio

and is

Maximum Change in Slope Ratio

and is

Click Calculate Flamelets to begin the diffusion flamelet calculation. Sample output for a flamelet

calculation is shown below.

Generating flamelet  at scalar dissipation  . /s

Time (s)   Temp (K)   Residual

.679e-   . .779e+

.038e-   . .734e-

.175e-   . .648e-

.519e-   . .652e-

.206e-   . .295e-

.058e-   . .100e+

.133e-   . .540e+

.282e-   . .607e+

.581e-   . .639e+

.718e-   . .905e+

.437e-   . .792e+

.877e-   . .659e+

.375e-   . .922e+

.751e-   . .181e+

.502e-   . .549e+

.100e+   . .639e+

.201e+   . .604e+

.402e+   . .307e+

.804e+   . .420e-

.761e+   . .581e-

.522e+   . .199e-

.043e+   . .735e-

.409e+   . .217e-

.817e+   . .892e-

.635e+   . .777e-

Flamelet successfully generated

In the Flamelet tab of the Species Model dialog box (Figure . : The Flamelet Tab for the Unsteady

Diffusion Flamelet Model (p. )), you will enter values for parameters of the flamelet.

Figure . : The Flamelet Tab for the Unsteady Diffusion Flamelet Model

The Unsteady Flamelet Parameters are as follows:

(

are solved coupled and implicit in  space, the solution time and memory requirements increase with

the number of  grid points.

Mixture Fraction Lower Limit for Initial Probability

is the mixture fraction above which the marker probability will be initialized to , and below which the

marker probability will be initialized to . In general, it should be set greater than the stoichiometric

mixture fraction.

Maximum Scalar Dissipation

is where flamelets extinguish at large scalar dissipation (mixing) rates.To prevent excessive mixing in the

flamelet, ANSYS Fluent allows you to specify a Maximum Scalar Dissipation rate for the 1D flamelet

equations. A reasonable value for this is the steady flamelet extinction scalar dissipation.The default value

of /s is near the steady extinction scalar dissipation of a methane-air flame at standard temperature

and pressure.

Courant Number

is the number at which ANSYS Fluent automatically selects the time step for the probability equation

based on this convective Courant number.

Number of Flamelets

is the number of unsteady laminar flamelets to be initiated in the simulation.The probability marker

equation will be solved for each flamelet.

Click Initialize Unsteady Flamelet Probability to initialize the unsteady flamelet and its probability

marker equation. ANSYS Fluent is now ready for postprocessing the 1D unsteady flamelet and the

2D/3D unsteady marker probability equation.

The flamelet tables may be written to a file for import into later sessions of ANSYS Fluent. You may

want to do this, for example, to change the number of discretization points in the PDF table, or to

plot the flamelet profiles in ANSYS Fluent. The flamelet tables should be saved before you create the

PDF table:

File → Write → Flamelet...

For the flamelet model, you can display or write flamelet curves. Click the Display Flamelets... or

PDF table:

Display Unsteady Flamelet... button. If you have a single flamelet, as for the unsteady diffusion

flamelet model, you can access the Flamelet 2D Curves dialog box (Figure . : The Flamelet 2D

curves Dialog Box (p. )).

Figure . : The Flamelet 2D curves Dialog Box

For the steady diffusion flamelet model with more than one flamelet, you can display 2D plots and

3D surfaces showing the variation of species fraction or temperature with the mean mixture fraction

or scalar dissipation using the Flamelet 3D Surfaces dialog box (for example, Figure . : The

Flamelet 3D Surfaces Dialog Box (p. )).

To access this dialog box, click the Display Flamelets... button in the Flamelet tab of the Species

Model dialog box, as shown in Figure . : The Species Model Dialog Box (Flamelet Tab) (p. ).

Figure . : The Flamelet 3D Surfaces Dialog Box

To display the flamelet tables graphically, use the following procedure:

. In the Flamelet 3D Surfaces dialog box, from the Plot Variable drop-down list, select the variable you

want to display graphically.

. Specify the Plot Type as either 3D Surface or 2D Curve on 3D Surface.

For a 3D surface, enable or disable Draw Numbers Box under Options.When this option is turned on,

the display will include a wireframe box with the numerical limits in each coordinate direction.

For a 2D curve on a 3D surface:

a.

Specify whether you want to write the plot data to a file by toggling Write To File under Options.

b. Specify the X-Axis Function against which the plot variable will be displayed by selecting Scalar

Dissipation ( ), or Mixture Fraction ( ).The variable that is not selected will be held constant.

c.

Specify the type of discretization (that is, how the flamelet data will be sliced) for the variable that

is being held constant (under Constant Value of Mixture Fraction or Constant Value of Scalar

Dissipation).

– If you selected Index under Slice by, specify the discretization Index of the variable that is being

held constant.The range of integer values that you are allowed to choose from is displayed under

Min and Max, and is equivalent to the number of points specified for that variable in the

Flamelet tab of the Species Model dialog box (see Calculating the Flamelets (p. )).

– If you selected Value under Slice by, specify the numerical Value of the variable that is being

held constant.The range of values that you can specify is displayed under Min and Max.

. Write or display the flamelet table results. If you have turned on the Write To File option for a 2D plot,

click Write and specify a name for the file in The Select File Dialog Box (p. ). Otherwise, click Plot or

Display as appropriate to display a 2D plot or 3D surface in the graphics window.

Figure . : Example 2D Plot of Flamelet Data (p. ) and Figure . : Example 3D Plot of Flamelet

Data (p. ) show examples of a 2D curve plot and 3D surface plot of a flamelet table.

Figure . : Example 2D Plot of Flamelet Data

Figure . : Example 3D Plot of Flamelet Data

ANSYS Fluent requires additional inputs that are used in the creation of the look-up tables. Several of

these inputs control the number of discrete values for which the look-up tables will be computed. These

parameters are input in the Table tab of the Species Model dialog box. When Automated Grid Refine-

ment is enabled, you will specify the table parameters displayed in Figure . : The Species Model

Dialog Box (Table) Tab Displaying Automated Grid Refinement (p. ). If Automated Grid Refinement

is disabled, you will specify the table parameters displayed in Figure . : The Species Model Dialog

Box (Table) Tab Excluding Automated Grid Refinement (p. ).

Note

Automated Grid Refinement is not available with two mixture fractions.

Calculating the Look-Up Tables

Figure . : The Species Model Dialog Box (Table) Tab Displaying Automated Grid Refinement

The look-up table parameters when Automated Grid Refinement is enabled are as follows:

Initial Number of Grid Points

specifies the number of grid points for the resolution of the mean mixture fraction, mixture fraction variance,

and mean enthalpy (for non-adiabatic systems).

Maximum Number of Grid Points

specifies the maximum number of grid points used for tabulation.The grid refinement procedure will stop

inserting the points when either the change in value and slope between successive points is within tolerance

or the maximum number of grid points are generated.

specifies the maximum allowable change in value of table variables between successive grid points as

specified by Equation . in the Theory Guide.

specifies the maximum change in the slope of table variables between successive grid points as specified

by Equation . in the Theory Guide.

Maximum Number of Species

is the maximum number of species stored in the lookup tables.

Figure . : The Species Model Dialog Box (Table) Tab Excluding Automated Grid Refinement

The look-up table parameters when Automated Grid Refinement is disabled are as follows:

Number of Mean Mixture Fraction Points

is the number of discrete values of  at which the look-up tables will be computed. For a two-mixture-

fraction model, this value is the number of points in the instantaneous state profile used to compute the

PDF if you choose the  PDF model (see Tuning the PDF Parameters for Two-Mixture-Fraction Calcula-

tions (p. )). Increasing the number of points will yield a more accurate PDF shape, but the calculation

will take longer.The mean mixture fraction points will be automatically clustered around the stoichiometric

mixture fraction value.

Number of Mixture Fraction Variance Points

is the number of discrete values of

at which the look-up tables will be computed. Lower resolution is

acceptable because the variation along the

axis is, in general, slower than the variation along the

axis of the look-up tables.This option is available only when no secondary stream has been defined.

Number of Secondary Mixture Fraction Points

at which the look-up tables will be computed. Like the Number

of Mean Mixture Fraction Points, ANSYS Fluent will use the Number of Secondary Mixture Fraction

Points to compute the equilibrium state-relation if you choose the  PDF option (see Tuning the PDF

Parameters for Two-Mixture-Fraction Calculations (p. )) for a two-mixture-fraction model. A larger

number of points will give a more accurate shape for the PDF, but with a longer calculation time.This

option is available only when a secondary stream has been defined.

is the maximum number of species that will be included in the look-up tables.The maximum number of

species that can be included is . ANSYS Fluent will automatically select the species with the largest

mole fractions to include in the PDF table. Note that the PDF table values of density and specific heat are

pre-calculated with all the species, and hence the convergence behavior of ANSYS Fluent will not be affected

by the input for the Maximum Number of Species. Hence, to keep table sizes small, you should set the

Maximum Number of Species to only include the species that you are interested in postprocessing.

Number of Mean Enthalpy Points

is the number of discrete values of enthalpy at which the look-up tables will be computed.This input is

required only if you are modeling a non-adiabatic system.The number of points required will depend on

the chemical system that you are considering, with more points required in high heat release systems (for

example, hydrogen/oxygen flames).This option is not available with the unsteady flamelet model.

Minimum Temperature

is used to determine the lowest temperature for which the look-up tables are generated.Your input should

correspond to the minimum temperature expected in the domain (for example, an inlet or wall temperature).

The minimum temperature should be set – K below the minimum system temperature.This option

is available only if you are modeling a non-adiabatic system.This option is not available with the unsteady

flamelet model.

Include Equilibrium Flamelet

specifies that an equilibrium flamelet (that is,

) will be generated in ANSYS Fluent and appended to

the flamelet library before the PDF table is calculated.This option is available when generating or importing

multiple flamelets, as well as when a single flamelet is considered. In the latter case, the PDF table will

consist of two scalar dissipation slices, namely the equilibrium slice at

, and the flamelet slice.This

option is available only with the steady diffusion flamelet model.

When you are satisfied with your inputs, click Calculate PDF Table to generate the look-up tables.

The computations performed for a single-mixture-fraction calculation culminate in the discrete integration

of Equation . (or Equation . in the Theory Guide) as represented in Figure . : Logical Dependence

of Averaged Scalars on Mean Mixture Fraction, the Mixture Fraction Variance, and the Chemistry Model

(Adiabatic, Single-Mixture-Fraction Systems) (or Figure . : Logical Dependence of Averaged Scalars on

Mean Mixture Fraction, the Mixture Fraction Variance, Mean Enthalpy, and the Chemistry Model (Non-

Adiabatic, Single-Mixture-Fraction Systems) in the Theory Guide). For a two-mixture-fraction calculation,

ANSYS Fluent will calculate the physical properties using Equation . or its adiabatic equivalent. The

computation time will be shortest for adiabatic single-mixture-fraction equilibrium calculations and

longest for non-adiabatic calculations involving multiple flamelet generation. Below, sample outputs

are shown for an adiabatic single-mixture-fraction equilibrium calculation and a non-adiabatic calculation

with flamelets:

Generating PDF lookup table

Type of the PDF Table: Adiabatic Table (Two Streams)

Calculating table .....

points calculated

species added

PDF Table successfully generated!

Type of the PDF Table: Nonadiabatic Table with Strained Flamelet Model (Two Streams)

calculating temperature limits .....

calculating scalar dissipation slices .....

scalar dissipation slice

calculating equilibrium slice .....

Performing PDF integrations.....

Initializing PDF table arrays and structures.

Important

Note that there is a significant difference in run time between the one-mixture fraction

model and the two-mixture fraction model. In the one-mixture fraction model, the PDF table

contains the mean data of density, temperature, and specific heats, and is three-dimensional

for an equilibrium nonadiabatic case (mean mixture fraction, mixture fraction variance, and

mean heat loss). For this case, ANSYS Fluent updates properties every flow iteration. In the

case of the two-mixture fraction model, only the instantaneous state relationships are stored

and mean properties are calculated from these by performing PDF integrations in every cell

of the ANSYS Fluent simulation. Since this is computationally expensive, ANSYS Fluent provides

the option of only updating properties after a specified number of iterations.

For a two-mixture fraction model, you can also refer to Full Tabulation of the Two-Mixture-

Fraction Model (p. ) for more information.

After completing the calculation at the specified number of mixture fraction points, ANSYS Fluent reports

that the calculation succeeded. In a single-mixture-fraction case, the resulting look-up tables take the

form illustrated in Figure . : Visual Representation of a Look-Up Table for the Scalar (Mean Value of

Mass Fractions, Density, or Temperature) as a Function of Mean Mixture Fraction and Mixture Fraction

Variance in Adiabatic Single-Mixture-Fraction Systems in the Theory Guide (or Figure . : Visual Repres-

entation of a Look-Up Table for the Scalar as a Function of Mean Mixture Fraction and Mixture Fraction

Variance and Normalized Heat Loss/Gain in Non-Adiabatic Single-Mixture-Fraction Systems, for non-

adiabatic systems). These look-up tables can be plotted using the available graphics tools, as described

in Postprocessing the Look-Up Table Data (p. ).

Note that in non-adiabatic calculations, the console window will report that the temperature limits and

enthalpy slices have been calculated.

For a two-mixture-fraction case, the resulting look-up tables take the form illustrated in Figure . : Visual

Representation of a Look-Up Table for the Scalar φ_I as a Function of Fuel Mixture Fraction and Secondary

Partial Fraction in Adiabatic Two-Mixture-Fraction Systems in the Theory Guide (or Figure . : Visual

Partial Fraction, and Normalized Heat Loss/Gain in Non-Adiabatic Two-Mixture-Fraction Systems, for

non-adiabatic systems).

... Full Tabulation of the Two-Mixture-Fraction Model

The default algorithm for the two-mixture-fraction model is to perform PDF integrations of the equi-

librium state relationships at run time. Since these are multi-dimensional integrals, the default two-

mixture-fraction model can be computationally demanding.

Alternatively, you may want to pre-compute these integrations and create 4D look-up tables for adia-

batic simulations, or 5D tables for non-adiabatic simulations. Such high-dimensional tables are compu-

tationally expensive to build, and may require large memory and disk storage, but can offer substantial

improvement in run time speed.

The option to create a fully-tabulated two-mixture-fraction table is available in cases with the two-

mixture-fraction model enabled, via the text command:

define/models/species/full-tabulation?

If you are modeling pollutant formation, note that the full tabulation option is not compatible with

the mixture-fraction option for PDF Mode in the Turbulence Interaction Mode tab settings. See

Setting Turbulence Parameters (p. ) for details on Turbulence Interaction options for pollutant

modeling.

modeling.

... Stability Issues in Calculating Chemical Equilibrium Look-Up Tables

Complex chemistry and non-adiabatic effects may make the equilibrium calculation more time-con-

suming and difficult. In some instances the equilibrium calculation may even fail. You may be able to

eliminate any difficulties that you encounter by trying the calculation as an adiabatic system. Adiabatic

system calculations are generally quite straightforward and can provide valuable insight into the op-

timal inputs to the non-adiabatic calculation.

Additional stability issues may arise for solid or heavy liquid fuels that have been defined using the

empirical fuel approach. You may find that, for rich fuel mixtures, the equilibrium calculation produces

very low temperatures and eventually fails. This indicates that strong endothermic reactions are taking

place and the mixture is not able to sustain them. In this situation, you may need to raise the heating

value of the fuel until ANSYS Fluent produces acceptable results. Provided that your fuel will be treated

as a liquid or solid (coal) fuel, you can maintain the desired heating value in your ANSYS Fluent simu-

lation. This is accomplished by defining the difference between the desired and the adjusted heating

values as latent heat (in the case of combusting solid fuel) or heat of pyrolysis (in the case of liquid

fuel).

... Saving the Look-Up Tables

The look-up tables may be stored in a file that you can read back into later sessions of ANSYS Fluent.

The look-up tables should be saved before you exit from the current ANSYS Fluent session.

File → Write → PDF...

By default, the file will be saved as formatted (ASCII, or text). To save a binary (unformatted) file, turn

on the Write Binary Files option in the Select File dialog box.

... Postprocessing the Look-Up Table Data

It is important for you to view your temperature and species tables to ensure that they are adequately

but not excessively resolved. Inadequate resolution will lead to inaccuracies, and excessive resolution

will lead to unnecessarily slow calculation times.

After a PDF table has been generated or read into ANSYS Fluent, you can display 2D plots and 3D

surfaces showing the variation of species mole fraction, density, or temperature with the mean mixture

fraction, mixture fraction variance, or enthalpy using the PDF Table dialog box (for example, Fig-

ure . : The PDF Table Dialog Box (Non-Adiabatic Case With Flamelets) (p. )). The PDF Table dialog

box can be accessed in one of two ways:

by clicking the Display PDF Table... button in the Table tab of the Species Model dialog box (as shown

in Figure . :The Species Model Dialog Box (Table) Tab Excluding Automated Grid Refinement (p. ))

by using the following path:

Postprocessing → Model Specific → PDF Table...

Figure . : The PDF Table Dialog Box (Non-Adiabatic Case With Flamelets)

To display the look-up tables graphically, use the following procedure:

. In the PDF Table dialog box, in the Plot Variable drop-down list you can select temperature, density, or

species mole fraction as the variable to be plotted.

. (multiple flamelets only) Specify the value of the Scalar Dissipation. In the case of non-adiabatic flamelets,

there is the additional parameter of mean enthalpy. In addition to varying the mean enthalpy and mean

mixture fraction, you can vary the display of the PDF table by changing the value of the scalar dissipation,

which gives the table a fourth “dimension”.

. Specify the Plot Type as either 3D Surface or 2D Curve on 3D Surface. In the equilibrium model, a 2D

curve is a slice of a 3D surface, and therefore some options selected for a 3D surface may impact the display

of a 2D curve.

For a 3D surface:

a.

Enable or disable Draw Numbers Box under Options.When this option is turned on, the display

will include a wireframe box with the numerical limits in each coordinate direction.

b. (non-adiabatic cases only) Under Surface Parameters, specify the discrete independent variable

to be held constant in the look-up table (Constant Value of).

– For a single-mixture-fraction case, select Scaled Heat Loss/Gain (

), Mean Mixture Fraction

( ), or Scaled Variance (

). For any mean mixture fraction , the variance varies between a

minimum of  and a maximum of

. In order to view the mixture fraction variance, it is

normalized by Equation . (p. ) so that for any mean mixture fraction the scaled variance

ranges from  to ..

(.)

– For a two-mixture-fraction case, the Scaled Heat Loss/Gain is the only available option.

c.

(non-adiabatic cases only) Specify whether the 3D array of data points available in the look-up table

will be sliced by Index or Value under Slice by.

– If you selected Index, specify the discretization Index of the variable that is being held constant.

The range of integer values that you are allowed to choose from is displayed under Min and Max,

and is equivalent to the number of points specified for that variable in the Table tab of the Species

Model dialog box (see Calculating the Look-Up Tables (p. )). If you specified to hold the enthalpy

(Scaled Heat Loss/Gain) constant, the enthalpy slice index corresponding to the adiabatic case

will be displayed in the Adiabatic field.

– If you selected Value, specify the numerical Value of the variable that is being held constant.The

range of values that you can specify is displayed under Min and Max.

a.

b. Under Curve Parameters, specify the X-Axis Function against which the plot variable will be dis-

played.

– For an adiabatic single-mixture-fraction case, select Mean Mixture Fraction ( ), or Scaled Variance

(

).

– For a non-adiabatic single-mixture-fraction case, the options will depend on what was selected

under Constant Value of under Surface Parameters, but will include two of the following: Scaled

Heat Loss/Gain (

), Mean Mixture Fraction, and Scaled Variance.

– For a two-mixture-fraction case, select Fuel Mixture Fraction (

) or Secondary Partial Fraction

(

).

c.

Specify the type of discretization (that is, how the look-up table data will be sliced) for the variable

that is being held constant (under Constant Value of Mean Mixture Fraction, Constant Value of

Scaled Variance, and so on). Note that for non-adiabatic cases, each 3D surface slice contains a full

set of 2D slices.

Min and Max, and is equivalent to the number of points specified for that variable in the Table

tab of the Species Model dialog box (see Calculating the Look-Up Tables (p. )).

. Write or display the look-up table results. If you have turned on the Write To File option for a 2D plot,

Figure . : Mean Species Mole Fraction Derived From an Equilibrium Chemistry Calculation (p. )

and Figure . : Mean Temperature Derived From an Equilibrium Chemistry Calculation (p. ) show

examples of 2D plots derived for a very simple hydrocarbon system.

Figure . : Mean Species Mole Fraction Derived From an Equilibrium Chemistry Calculation

Figure . : Mean Temperature Derived From an Equilibrium Chemistry Calculation

Figure . : 3D Plot of Look-Up Table for Temperature Generated for a Simple Hydrocarbon Sys-

tem (p. ) shows an example of a 3D surface derived for the same system.

Figure . : 3D Plot of Look-Up Table for Temperature Generated for a Simple Hydrocarbon

System

The standard flamelet file format can be used to read and write non-premixed (diffusion) flamelets. The

data structure for the standard flamelet file format is based on keywords that precede each data section.

If any of the keywords in your flamelet data file do not match the supported keywords, you will have

to manually edit the file and change the keywords to one of the supported types. (The ANSYS Flu-

ent flamelet filter is case-insensitive, so you need not worry about capitalization within the keywords.)

The following keywords are supported by the ANSYS Fluent filter:

Keyword

HEADER

Header section

BODY

Main body section

NUMOFSPECIES

Number of species

GRIDPOINTS

Number of grid points

PRESSURE

Pressure

STRAINRATE

Strain rate for diffusion flamelet generated in

physical space

STOICH_SCADIS or CHI

Stoichiometric scalar dissipation for diffusion

flamelet

STOICH_Z

Stoichiometric mixture fraction

TEMPERATURE and TEMP

MASSFRACTION-

Mass fraction

Z

Mixture fraction

MOLEFRACTION-

Mole fraction

Note

The strain rate output is written if the flamelets are generated in physical space, for example,

using ANSYS CHEMKIN.

... Sample Standard Diffusion Flamelet File

A sample diffusion flamelet file in the standard format is provided below. Note that not all species are

listed in this file.

HEADER

STOICH_SCADIS   .000000E-

STOICH_Z        .618652E-

HEADER

PRESSURE        .013250E+

BODY

Z

.000000000E+ .273315430E- .240997314E- .447830200E- .551246643E-

.602954865E- .654663086E- .068328857E- .481994629E- .309326172E-

.136657715E- .963989258E- .377655029E- .791320801E- .204986572E-

.618652344E- .912528540E- .206404735E- .500280931E- .794157127E-

.867626176E- .941095225E- .088033323E- .381909519E- .675785714E-

.969661910E- .263538106E- .557414302E- .014516669E- .073291909E-

.132067148E- .190842387E- .249617626E- .367168104E- .425943343E-

.484718583E- .543493822E- .572881441E- .602269061E- .672799348E-

Standard Files for Diffusion Flamelet Modeling

.743329635E- .884390209E- .166511357E- .448632505E- .730753653E-

.407844408E- .084935163E- .709952975E- .659974350E- .000000000E+

TEMPERATURE

.000000000E+ .268546798E+ .802882604E+ .544333704E+ .908936814E+

.089771589E+ .269654154E+ .067550740E+ .203418117E+ .462664100E+

.707202552E+ .934669997E+ .037622483E+ .128475386E+ .200397351E+

.244572249E+ .254177637E+ .245072250E+ .220638695E+ .186735136E+

.177535664E+ .168109526E+ .148737393E+ .108856496E+ .068758176E+

.029154219E+ .990673114E+ .953782923E+ .885112633E+ .821857119E+

.761797286E+ .703540208E+ .647197627E+ .543457773E+ .496624533E+

.452642813E+ .410968313E+ .390849359E+ .371237774E+ .326602075E+

.286669965E+ .222176660E+ .134221753E+ .064763074E+ .004219101E+

.845385948E+ .871510772E+ .152847269E+ .605312740E+ .000000000E+

massfraction-h

.000000000E+ .470246609E- .689876963E- .823505733E- .604836416E-

.259465253E- .137901769E- .297692554E- .299314819E- .009221085E-

.364446760E- .504321512E- .488600091E- .041919731E- .259044043E-

.764854561E- .446982906E- .948355957E- .067005444E- .858096141E-

.763204904E- .660609671E- .447858861E- .024662524E- .571691024E-

.207106883E- .769042791E- .144795604E- .683704776E- .862438419E-

.529575950E- .577642294E- .493198194E- .597224020E- .397461608E-

.672683885E- .109095223E- .352078253E- .847760877E- .024498078E-

.804126487E- .241975019E- .664800458E- .824650210E- .058872219E-

.103611172E- .070333150E- .521048377E- .116361056E- .000000000E+

massfraction-o2

.330000000E- .037872969E- .891809523E- .818777426E- .782261116E-

.764002861E- .745744526E- .599674402E- .453586904E- .161277458E-

.685446531E- .764270922E- .337649028E- .986903537E- .792882492E-

.656537748E- .260825775E- .718417261E- .787962652E- .809733781E-

.319197735E- .626119601E- .195145104E- .624530279E- .000207346E-

.625791857E- .935574928E- .314963476E- .242565474E- .388575920E-

.396692299E- .701489188E- .617025651E- .172983452E- .146818725E-

.500353242E- .052693603E- .680804793E- .032480088E- .785587351E-

.627110024E- .631110236E- .316226342E- .904385354E- .159316969E-

.851864505E- .569901388E- .016058744E- .304158252E- .000000000E+

massfraction-oh

. . . . .

. . . . .

. . . . .

... Missing Species

ANSYS Fluent will check whether all species in the flamelet data file exist in the thermodynamic

properties databases thermo.db. If any of the species in the flamelet file do not exist, ANSYS Fluent will

issue an error message and halt the flamelet import. If this occurs, you can either add the missing

species to the database, or remove the species from the flamelet file.

You should not remove a species from the flamelet data file unless its species concentration is very

small (- or less) throughout the flamelet profile. If you remove a low-concentration species, you will

not have the species concentrations available for viewing in the ANSYS Fluent calculation, but the ac-

curacy of the ANSYS Fluent calculation will otherwise be unaffected.

Important

If you choose to remove any species, be sure to also update the number of species (keyword

NUMOFSPECIES) in the flamelet data file, to reflect the loss of any species you have removed

from the file.

If a species with relatively large concentration is missing from the ANSYS Fluent thermodynamic

databases, you will have to add it. Removing a high-concentration species from the flamelet file is not

This section describes how to set up and apply the inert model. For a discussion about the theory, refer

to Using the Non-Premixed Model with the Inert Model in the Theory Guide.

To enable the inert model, make sure that the non-premixed or partially premixed model is selected in

the Species Model dialog box, or that a PDF file is read. Refer to Steps in Using the Non-Premixed

Model (p. ) and Modeling Partially Premixed Combustion (p. ) to learn more about these models.

Setup → Models → Inert

Edit...

Figure . : The Inert Model Dialog Box

The Inert dialog box will be displayed (Figure . : The Inert Model Dialog Box (p. )). To enable this

Edit...

model, select Inert Transport. The following steps will walk you through setting up the inert model:

. Select Fixed H/C Ratio as the Composition Option if the hydrogen to carbon ratio is known. For example,

for methane (CH4) enter  for H/C Ratio.

Setting the H/C ratio assumes that the burned gas resulted from the complete, stoichiometric

combustion of that hydrocarbon fuel with air, and the only products of the combustion are CO2,

H2O and N2.

. Select User Specified as the Composition Option if you want to specify an arbitrary composition for the

inert stream, as shown in Figure . :The Inert Model Dialog Box (p. ).

Setting Up the Inert Model

You can specify your composition stream by adding or removing species if your stream is composed

of species other than the default species list.

a.

To add species to the Species list, type the chemical formula under Inert Species and click Add.

b. Enter the Mass Fraction of the newly added species. Continue in this manner until all of the inert species

you want to include are shown in the Species list.

c.

Make sure the sum of the mass fractions add up to . ANSYS Fluent will normalize the species mass

fractions for you when you click Normalize Species.

d. To remove a species from the list, type the chemical formula under Inert Species and click Remove.

e. To print a list of all species in the thermodynamic database file (thermo.db) in the console window,

click List Available Species.

... Setting Boundary Conditions for Inert Transport

You will need to set appropriate boundary conditions at flow inlets and exits for the inert tracer mass

fraction,

. The tracer species mass fraction must be between zero and one, with the value of one

meaning that all of the material entering the domain comes from the inert stream. The values for flow

boundaries are set in the Inert Stream field of the inlet boundary condition dialog boxes, under the

Species tab.

... Initializing the Inert Stream

The main assumption of the inert model is that the composition of the inert stream does not change

with combustion. For some dilutants, this is a very reasonable assumption, however, it is not valid for

rich combustion where there is fuel in the exhaust stream. For cases where there is fuel or oxidizer

left in the exhaust gas, the accuracy of your results will depend upon taking the fuel or oxidizer species

into account when setting initial conditions.

.... Inert Fraction

Initialization of the inert mass fraction

is done in the same way as other variables: by entering in

the appropriate value in the Solution Initialization task page. Another option for initialization is to

patch the value of

in a region of the domain. When the value of

is patched in this way, ANSYS

Fluent automatically recalculates the enthalpy field for the current temperature field in order to account

for the change in composition.

See Patching Values in Selected Cells (p. ) for details about patching values of solution variables.

.... Inert Composition

For combustion calculations that burn a hydrocarbon fuel, ANSYS Fluent provides a straightforward

way of setting the initial composition of the inert stream. The inert composition can be set by assuming

a ratio of hydrogen to carbon in the following overall oxidation reaction (from Heywood [] (p. )):

(.)

which can be rewritten in terms of the ratio of hydrogen to carbon atoms (

) in the fuel as

(.)

If Equation . (p. ) is solved for the mass fractions of CO2, H2O and N2, the following relations

are obtained:

(.)

where

Setting the H/C ratio assumes that the burned gas resulted from the complete, stoichiometric com-

bustion of that hydrocarbon fuel, and the only products of the combustion are CO2, H2O and N2. An

arbitrary composition for the inert stream can also be specified in the interface.

... Resetting Inert EGR

ANSYS Fluent allows burned gases to be converted to an inert gas. This has been designed with in-

cylinder combustion in mind to aid the simulation of multiple cycles of such engines using the partially-

premixed combustion model with exhaust gas recirculation (EGR). At the end of a combustion stroke,

the premixed progress variable of the burnt gases is unity. When fresh charge, with progress variable

of zero, is mixed with the burnt trapped gases, combustion will be initiated unless these trapped gases

are converted to inert.

This facility is accessed via the Dynamic Mesh Events dialog box, as described in Resetting Inert

EGR (p. ). There, you will need to set the crank angle at which the event occurs (usually shortly before

the inlet valves open) and at the fluid zones (usually the combustion chamber) where the burnt gases

When ANSYS Fluent performs an inert reset, the inert composition is calculated as the stoichiometric

composition. For lean mixtures, the stoichiometric inert is mixed with oxidizer, and for rich mixtures

the stoichiometric inert is mixed with fuel, so that overall stoichiometry is conserved. This entails:

Calculating the stoichiometric mixture fraction, which is defined as the mixture where both fuel and

oxidizer are completely consumed.

Calculating the inert species mass fractions as the stoichiometric species mass fractions. Species with

mole fractions less than . are discarded.

Setting the inert mass fraction and the mixture fraction as follows:

– Lean mixtures

– Rich mixtures

where

is the inert mass fraction,

is the mixture fraction,  is the reaction progress, sub-

script sto denotes stoichiometric, subscript old denotes values before inert reset, tilde super-

script denotes Favre averaging.

Setting the reaction progress to zero.

– For the ECFM model, flame area density is set to zero.

– For the G-Equation model, G (the mean distance from the flame front) is set to a negative value.

Since there will be some small errors in the species mass fractions from before the EGR reset, the

temperature will change due to the change in the specific heat. By default, ANSYS Fluent adjusts the

enthalpy so that temperature is unchanged after EGR reset.This may be limited by the PDF table

temperature limits for the new mixture fraction, in which case the temperature after inert reset will

not equal the temperature before the inert reset event.

For information about defining non-premixed boundary conditions, see the following sections:

... Input of Mixture Fraction Boundary Conditions

... Diffusion at Inlets

... Input of Thermal Boundary Conditions and Fuel Inlet Velocities

When the non-premixed combustion model is used, flow boundary conditions at inlets and exits (that

is, velocity or pressure, turbulence intensity) are defined in the usual way. Species mass fractions at

inlets are not required. Instead, you define values for the mean mixture fraction,

, and the mixture

fraction variance,

, at inlet boundaries. (For problems that include a secondary stream, you will

define boundary conditions for the mean secondary partial fraction and its variance as well as the

mean fuel mixture fraction and its variance.) These inputs provide boundary conditions for the conser-

vation equations you will solve for these quantities. The inlet values are supplied in the boundary

conditions task page, under the available tabs, for the selected inlet boundary (for example, Fig-

ure . : The Velocity Inlet Dialog Box Showing Mixture Fraction Boundary Conditions (p. )).

Setup →

Figure . : The Velocity Inlet Dialog Box Showing Mixture Fraction Boundary Conditions

Click the Species tab and specify the Mean Mixture Fraction and Mixture Fraction Variance (and

the Secondary Mean Mixture Fraction and Secondary Mixture Fraction Variance, if you are using

two mixture fractions). In general, the inlet value of the mean fractions will be . or . at flow inlets:

the mean fuel mixture fraction will be . at fuel stream inlets and . at oxidizer or secondary stream

inlets; the mean secondary mixture fraction will be . at secondary stream inlets and . at fuel or

oxidizer inlets. The fuel or secondary mixture fraction will lie between . and . only if you are

Defining Non-Premixed Boundary Conditions

modeling flue gas recycle, as illustrated in Figure . : Using the Non-Premixed Model with Flue Gas

Recycle and discussed in Definition of the Mixture Fraction in the Theory Guide. The fuel or secondary

mixture fraction variance can usually be taken as zero at inlet boundaries.

In some cases, you may want to include the diffusive transport of mixture fraction through the inlets

of your domain. You can do this by enabling inlet mixture-fraction diffusion. By default, ANSYS Flu-

ent excludes the diffusion flux of mixture fraction at inlets. To enable inlet diffusion, use either the

define/models/ species/inlet-diffusion?

text command, or the Species Model dialog box (Figure . : Defining Equilibrium Chemistry (p. ))

Edit...

and enable the Inlet Diffusion option.

If your model is non-adiabatic, you should specify the Temperature at the flow inlets. Recall that the

inlet temperatures were requested during the table construction in the Chemistry tab of the Species

Model dialog box, and were used in the construction of the look-up tables. The inlet temperatures for

each fuel, oxidizer, and secondary inlet in your non-adiabatic model should be defined, in addition,

as boundary conditions in ANSYS Fluent. It is acceptable for the inlet temperature boundary conditions

to differ slightly from those you input for the look-up table calculations. If the inlet temperatures differ

significantly from those in the Chemistry tab, however, your look-up tables may provide inaccurate

interpolation. This is because the discrete points in the look-up tables were clustered around a finite

range of the temperatures defined in the Chemistry tab, and your input in the ANSYS Fluent inlet

boundary condition may fall outside this range.

Wall thermal boundary conditions should also be defined for non-adiabatic non-premixed combustion

calculations. You can use any of the standard conditions available in ANSYS Fluent, including specified

wall temperature, heat flux, external heat transfer coefficient, or external radiation. If radiation is to be

included within the domain, the wall emissivity should be defined as well. See Thermal Boundary

Conditions at Walls (p. ) for details about thermal boundary conditions at walls.

When you use the non-premixed combustion model, the material used for all fluid zones is automatically

set to pdf-mixture. This material is a special case of the mixture material concept discussed in Mixture

Materials (p. ). The constituent species of this mixture are the species that were calculated in the PDF

look-up table creation; you cannot change them directly. When the non-premixed model is used, heat

capacities, molecular weights, and enthalpies of formation for each species considered are extracted

from the chemical database, so you will not modify any properties for the constituent species in the

PDF mixture. For the PDF mixture itself, the mean density and mean specific heat are determined from

the look-up tables.

The physical property inputs for a non-premixed combustion problem are therefore only the transport

properties (viscosity, thermal conductivity, and so on) for the PDF mixture. To set these in the Create/Edit

Materials Dialog Box (p. ), choose mixture as the Material Type, pdf-mixture (the default, and only

choice) in the Mixture Materials list, and set the desired values for the transport properties.

Setup →

Materials

See Physical Properties (p. ) for details about setting physical properties. The transport properties in

a non-premixed combustion problem can be defined as functions of temperature, if desired, but not

as functions of composition. In practice, since turbulence effects will dominate, it will be of little benefit

to include even the temperature dependence of the laminar transport properties.

If you are modeling radiation heat transfer, you will also enter radiation properties, as described in Ra-

diation Properties (p. ). Composition-dependent absorption coefficients (using the WSGGM) are allowed.

The non-premixed model can also be used with real gas models in ANSYS Fluent, if the Compressibility

Effects option is enabled in the Species Model dialog box. In this case, the density method is based

on one of the four real gas models, discussed in Equation of State (p. ) and Using the Cubic Equation

of State Real Gas Models (p. ).

The non-premixed model setup and solution procedure in ANSYS Fluent differs slightly for single- and

two-mixture-fraction problems. Below, an overview of each approach is provided. Note that your ANSYS

Fluent case file must always meet the restrictions listed for the non-premixed modeling approach in

Restrictions on the Mixture Fraction Approach in the Theory Guide. In this section, details are provided

regarding the problem definition and calculation procedures you follow in ANSYS Fluent.

... Single-Mixture-Fraction Approach

...Two-Mixture-Fraction Approach

... Starting a Non-Premixed Calculation From a Previous Case File

... Solving the Flow Problem

For a single-mixture-fraction system, when you have completed the calculation of the PDF look-up

tables, you are ready to begin your reacting flow simulation. In ANSYS Fluent, you will solve the flow

field and predict the spatial distribution of  and

(and

if the system is non-adiabatic or  if the

system is based on laminar flamelets). ANSYS Fluent will obtain the corresponding values of temperature

and individual chemical species mass fractions from the look-up tables.

When a secondary stream is included, ANSYS Fluent will solve transport equations for the mean sec-

ondary partial fraction (

) and its variance in addition to the mean fuel mixture fraction and its

variance. ANSYS Fluent will then look up the instantaneous values for temperature, density, and indi-

vidual chemical species in the look-up tables, compute the PDFs for the fuel and secondary streams,

and calculate the mean values for temperature, density, and species.

Note that in order to avoid both inaccuracies and unnecessarily slow calculation times, it is important

for you to view your temperature and species tables in ANSYS Fluent to ensure that they are adequately

but not excessively resolved.

Solution Strategies for Non-Premixed Modeling

You can read a previously defined ANSYS Fluent case file as a starting point for your non-premixed

combustion modeling. If this case file contains inputs that are incompatible with the current non-

premixed combustion model, ANSYS Fluent will alert you when the non-premixed model is turned on

and it will turn off those incompatible models. For example, if the case file includes species that differ

from those included in the PDF file created by ANSYS Fluent, these species will be disabled. If the case

file contains property descriptions that conflict with the property data in the chemical database, these

property inputs will be ignored.

Important

PDF files created by prePDF  or older are not supported by this version of ANSYS Fluent.

The files generated by PrePDF version  or newer, are fully compatible.

In the Species Model dialog box, select Non-Premixed Combustion under the Model heading. When

you click OK in the Species Model dialog box, The Select File Dialog Box (p. ) will immediately appear,

prompting you for the name of the PDF file containing the look-up tables created in a previous ANSYS

Fluent session. (The PDF file is the file you saved using the File/Write/PDF... ribbon tab item after

computing the look-up tables.) ANSYS Fluent will indicate that it has successfully read the specified

PDF file:

Reading "/home/mydirectory/adiabatic.pdf"...

read  species (binary c, adiabatic fluent)

pdf file successfully read.

Done.

After you read in the PDF file, ANSYS Fluent will inform you that some material properties have changed.

You can accept this information; you will be updating properties later on.

You can read in an altered PDF file at any time by using the File/Read/PDF... ribbon tab item.

Important

Recall that the non-premixed combustion model is available only when you used the pres-

sure-based solver; it cannot be used with the density-based solvers. Also, the non-premixed

combustion model is available only when turbulence modeling is active.

If you are modeling a non-adiabatic system and you want to include the effects of compressibility, re-

open the Species Model dialog box and turn on Compressibility Effects under PDF Options. This

option tells ANSYS Fluent to update the density according to Equation . (p. ). When the non-

premixed combustion model is active, you can enable compressibility effects only in the Species

Model dialog box. For other models, you will specify compressible flow (ideal-gas, boussinesq, and

so on) in the Create/Edit Materials dialog box. See Specifying the Operating Pressure for the Sys-

tem (p. ) and Tuning the PDF Parameters for Two-Mixture-Fraction Calculations (p. ) for more

information about compressibility effects.

.... Retrieving the PDF File During Case File Reads

The PDF filename is specified to ANSYS Fluent only once. Thereafter, the filename is stored in your

ANSYS Fluent case file and the PDF file will be automatically read into ANSYS Fluent whenever the

case file is read. ANSYS Fluent will remind you that it is reading the PDF file after it finishes reading

the rest of the case file by reporting its progress in the text (console) window.

Note that the PDF filename stored in your case file may not contain the full name of the directory in

which the PDF file exists. The full directory name will be stored in the case file only if you initially

read the PDF file through the GUI (or if you typed in the directory name along with the filename

when using the text interface). In the event that the full directory name is absent, the automatic

reading of the PDF file may fail (since ANSYS Fluent does not know which directory to look in for the

file), and you will need to manually specify the PDF file. The safest approaches are to use the GUI

when you first read the PDF file or to supply the full directory name when using the text interface.

The next step in the non-premixed combustion modeling process in ANSYS Fluent is the solution of

the mixture fraction and flow equations. First, initialize the flow. By default, the mixture fraction and

its variance have initial values of zero, which is the recommended value; you should generally not set

nonzero initial values for these variables. See Initializing the Solution (p. ) for details about solution

Solution →

Next, begin calculations in the usual manner.

Solution →

Run Calculation

During the calculation process, ANSYS Fluent reports residuals for the mixture fraction and its variance

in the fmean and fvar columns of the residual report:

iter       cont       x-vel       y-vel          k     epsilon       fmean       fvar

.57e-     .92e-     .80e-    .68e-     .59e-     .09e-    .17e+

.42e-     .43e-     .23e-    .48e-     .30e-     .89e-    .15e+

.28e-     .98e-     .75e-    .29e-     .04e-     .88e-    .14e+

(For two-mixture-fraction calculations, columns for psec and pvar will also appear.)

.... Under-Relaxation Factors for PDF Equations

The transport equations for the mean mixture fraction and mixture fraction variance are quite stable

and high, under-relaxation can be used when solving them. By default, an under-relaxation factor of

is used for the mean mixture fraction (and secondary partial fraction) and . for the mixture fraction

variance (and secondary partial fraction variance). If the residuals for these equations are increasing,

you should consider decreasing these under-relaxation factors, as discussed in Setting Under-Relaxation

Factors (p. ).

solution. ANSYS Fluent allows you to under-relax the change in density to alleviate this difficulty. The

default value for density under-relaxation is , but if you encounter convergence trouble you may

want to reduce this to a value between . and  (in the Solution Controls task page).

....Tuning the PDF Parameters for Two-Mixture-Fraction Calculations

For cases that include a secondary stream, the PDF integrations are performed inside ANSYS Fluent.

The parameters for these integrations are defined in the Species Model Dialog Box (p. ) (Fig-

ure . : The Species Model Dialog Box for a Two-Mixture-Fraction Calculation (p. )).

Edit...

Figure . : The Species Model Dialog Box for a Two-Mixture-Fraction Calculation

The parameters are as follows:

Compressibility Effects

(non-adiabatic systems only) tells ANSYS Fluent to update the density, temperature, species mass fraction,

and enthalpy from the PDF tables to account for the varying pressure of the system.

The final step in the non-premixed combustion modeling process is the postprocessing of species

concentrations and temperature data from the mixture fraction and flow-field solution data. The following

variables are of particular interest:

Mean Mixture Fraction (in the Pdf... category)

Secondary Mean Mixture Fraction (in the Pdf... category)

Mixture Fraction Variance (in the Pdf... category)

Secondary Mixture Fraction Variance (in the Pdf... category)

Fvar Prod (in the Pdf... category, which is the production term in the mixture fraction variance transport

equation)

Fvar2 Prod (in the Pdf... category)

Scalar Dissipation (in the Pdf... category)

PDF Table Adiabatic Enthalpy (in the Pdf... category)

PDF Table Heat Loss/Gain (in the Pdf... category)

Mass fraction of species-n  (in the Species... category)

Mole fraction of species-n  (in the Species... category)

Molar Concentration of species-n  (in the Species... category)

RMS species-n Mass Fraction (in the Species... category)

Static Temperature (in the Temperature... category)

RMS Temperature (in the Temperature... category)

Enthalpy (in the Temperature... category)

Probability (in the Unsteady Flamelet... category)

Mean Temperature (in the Unsteady Flamelet... category)

Mean Mass Fraction of species-n  (in the Unsteady Flamelet... category)

Important

For the unsteady diffusion flamelet model, mean species mass fractions are displayed for the

first fifty species in the flamelet kinetic mechanism.

These quantities can be selected for display in the indicated category of the variable-selection drop-

down list that appears in postprocessing dialog boxes. See Field Function Definitions (p. ) for their

definitions.

In all cases, the species concentrations are derived from the mixture fraction/variance field using the

look-up tables. Note that temperature and enthalpy can be postprocessed even when your ANSYS Fluent

model is an adiabatic non-premixed combustion simulation in which you have not solved the energy

equation. In both the adiabatic and non-adiabatic cases, the temperature is derived from the look-up

table.

Figure . : Predicted Contours of Mixture Fraction in a Methane Diffusion Flame (p. ) and Fig-

ure . : Predicted Contours of CO2 Mass Fraction Using the Non-Premixed Combustion Model (p. )

illustrate typical results for a methane diffusion flame modeled using the non-premixed approach.

Postprocessing the Non-Premixed Model Results

Figure . : Predicted Contours of Mixture Fraction in a Methane Diffusion Flame

Figure . : Predicted Contours of CO2 Mass Fraction Using the Non-Premixed Combustion

Model

... Postprocessing for Inert Calculations

ANSYS Fluent provides several additional reporting options for post-processing calculations with the

inert model. You can generate graphical plots or alphanumeric reports of the same items that are

available with the non-premixed or partially premixed models, and in addition the following variables

are available:

Pdf Fmean

Pdf Fmean

Pdf Fvar

Mass Fraction of Inert

where the mass fraction of the

th inert species,

, is calculated as

where

is the inert tracer and

is the mass fraction of the

th inert species defined in the Inert

Note these variables appear in the Inert... category.

Chapter : Modeling Premixed Combustion

This chapters discusses how to simulate premixed turbulent combustion in ANSYS Fluent. For theoret-

ical background on this model, see Premixed Combustion in the Theory Guide.

Information about using this model is provided in the following sections:

.. Limitations of the Premixed Combustion Model

.. Using the Premixed Combustion Model

.. Setting Up the C-Equation and G-Equation Models

.. Setting Up the Extended Coherent Flame Model

.. Postprocessing for Premixed Combustion Calculations

The following limitations apply to the premixed combustion model:

You must use the pressure-based solver.The premixed combustion model is not available with the density-

based solver.

The premixed combustion model is valid only for turbulent, subsonic flows.These types of flames are called

deflagrations. Explosions, also called detonations, where the combustible mixture is ignited by the heat

behind a shock wave, can be modeled with the finite-rate model using the density-based solver. See Mod-

eling Species Transport and Finite-Rate Chemistry (p. ) for information about the finite-rate model.

The premixed combustion model cannot be used in conjunction with the pollutant (that is, soot and NOx)

models. However, a perfectly premixed system can be modeled with the partially premixed model (see

Modeling Partially Premixed Combustion (p. )), which can be used with the pollutant models.

You cannot use the premixed combustion model to simulate reacting discrete-phase particles, because

these would result in a partially premixed system. Only inert particles can be used with the premixed com-

bustion model.

The G-Equation model can be used only with the unsteady solver because it tracks the flame front in time.

However, RANS solutions, which tend to a steady-state, can be modeled by evolving them in time until the

solution is stationary.

The procedure for setting up and solving a premixed combustion model is outlined below, and then

described in detail. Remember that only the steps that are pertinent to premixed combustion modeling

are shown here. For information about inputs related to other models that you are using in conjunction

with the premixed combustion model, see the appropriate sections for those models.

.

Enable the premixed turbulent combustion model and set the related parameters.

Note

Make sure a turbulence model (other than the Spalart-Allmaras model) is selected before

selecting a combustion model.

Edit...

.

Define the physical properties for the unburnt and burnt material in the domain.

Setup →

.

Set the value of the progress variable  at flow inlets and exits.

Setup →

.

Initialize and patch the value of the progress variable.

Solution →

Initialization →

Patch...

.

Setup →

.

Solution →

Patch...

.

Solve the problem and perform postprocessing.

Important

If you are interested in computing the concentrations of individual species in the domain,

you can use the partially premixed model described in Modeling Partially Premixed Combus-

tion (p. ). Alternatively, compositions of the unburnt and burnt mixtures can be obtained

from external analyses using equilibrium or kinetic calculations.

... Enabling the Premixed Combustion Model

... Choosing an Adiabatic or Non-Adiabatic Model

To enable the premixed combustion model, select Premixed Combustion under Model in the Species

Model Dialog Box (p. ) (Figure . : The Species Model Dialog Box for Premixed Combustion (p. )).

Edit...

Modeling Premixed Combustion

Figure . : The Species Model Dialog Box for Premixed Combustion

When you enable Premixed Combustion, the dialog box expands to show the relevant inputs.

Under Premixed Combustion Model Options in the Species Model Dialog Box (p. ), choose either

Adiabatic (the default) or Non-Adiabatic. This choice affects only the calculation method used to

determine the temperature (either Equation . or Equation . in the Theory Guide).

When C Equation or G Equation is selected as the Premixed Model, you can then choose to use the

zimont or peters Flame Speed Model (described in Turbulent Flame Speed Models). You can also

modify a number of model constants, as described in Modifying the Constants for the Zimont Flame

Speed Model (p. ) and Modifying the Constants for the Peters Flame Speed Model (p. ).

Setting Up the C-Equation and G-Equation Models

Figure . : The Species Model Dialog Box for the G-Equation Model

For a non-adiabatic premixed combustion model, note that the value you specify for the Turbulent

Schmidt Number will also be used as the Prandtl number for energy. (The Energy Prandtl Number

will therefore not appear in the Viscous Model dialog box for non-adiabatic premixed combustion

models.) These parameters control the level of diffusion for the progress variable and for energy. The

progress variable is closely related to energy (because the flame progress results in heat release), so it

is important that the transport equations use the same level of diffusion.

... Modifying the Constants for the Zimont Flame Speed Model

... Modifying the Constants for the Peters Flame Speed Model

... Additional Options for the G-Equation Model

... Defining Physical Properties for the Unburnt Mixture

... Setting Boundary Conditions for the Progress Variable

... Initializing the Progress Variable

In general, you will not need to modify the constants used in the equations presented in C-Equation

Model Theory in the Theory Guide. The default values are suitable for a wide range of premixed flames.

You can set the Turbulent Length Scale Constant (

in Equation . ), Turbulent Flame Speed

Constant (  in Equation . ), the Stretch Factor Coefficient (

in Equation . ), the Turbulent

Schmidt Number (

in Equation . ), and the Wall Damping Coefficient (

in Equation . ).

The Peters turbulent flame speed model constants, as described in Peters Flame Speed Model in the

Theory Guide, are not available in the GUI because they are generally suitable for a wide range of

premixed flames. They can, however, be accessed from the TUI.

The Ewald Corrector is enabled by default and described in Peters Flame Speed Model. The Turbulent

in Equation .) are

the same as those described for the Zimont model.

When the G-Equation model is enabled, the G Equation Settings group box appears. You can select

either the transport equation or algebraic option for the calculation of the flame distance variance.

Consult Peters Flame Speed Model in the Theory Guide for the variance transport and algebraic

equation expressions (Equation . and Equation . ). It is recommended that you use the transport

equation option for RANS and the algebraic option for LES.

When Flame Curvature Source is enabled, the curvature source term in the G-Equation, which is the

last term in Equation ., is included. By default, this term is excluded.

The fluid material in your domain should be assigned the properties of the unburnt mixture, including

the thermal diffusivity (  in Equation . in the Theory Guide).

, and values at

standard conditions can be found in combustion handbooks (for example, [] (p. )).

For both adiabatic and non-adiabatic combustion models, you will need to specify the Laminar Flame

Speed (

in Equation . in the Theory Guide) as a material property, in the Create/Edit Materials

dialog box. You may choose to enter a constant value, use a user-defined function, or apply the

metghalchi-keck-law. See Laminar Flame Speed in the Theory Guide and Defining Physical Properties

for the Unburnt Mixture (p. ) for information about setting the other properties for the unburnt

material.

When using the Zimont turbulent flame speed model, if you want to include the flame stretch effect

in your model, you will also need to specify a lower value than the default Critical Rate of Strain (

in Equation . in the Theory Guide). As discussed in Flame Stretch Effect in the Theory Guide,

is

set to a very high value (

) by default, so no flame stretching occurs. To include flame

stretching effects, you will need to adjust the Critical Rate of Strain based on experimental data for

the burner. Because the flame stretching and flame extinction can influence the turbulent flame speed

(as discussed in Flame Stretch Effect in the Theory Guide), a realistic value for the Critical Rate of

Strain is required for accurate predictions. Typical values for

lean premixed combustion range

from  to

from  to

[] (p. ). Note that you can specify constant values or user-defined functions

to define the Laminar Flame Speed and Critical Rate of Strain. See the Fluent Customization

Manual for details about user-defined functions.

For adiabatic models, you will also specify the Adiabatic Burnt Temperature (

the Theory Guide), which is the temperature of the burnt products under adiabatic conditions. This

temperature will be used to determine the linear variation of temperature in an adiabatic premixed

combustion calculation. You can specify a constant value or use a user-defined function.

For non-adiabatic models, you will instead specify the Heat of Combustion per unit mass of fuel and

the Unburnt Fuel Mass Fraction (

and

in Equation . in the Theory Guide). ANSYS Flu-

ent will use these values to compute the heat losses or gains due to combustion, and include these

losses/gains in the energy equation that it uses to calculate temperature. The Heat of Combustion

can be specified only as a constant value, but you can specify a constant value or use a user-defined

function for the Unburnt Fuel Mass Fraction.

To specify the density for a premixed combustion model, choose premixed-combustion in the

Density drop-down list and set the Adiabatic Unburnt Density and Adiabatic Unburnt Temperature

(

and

in Equation . in the Theory Guide). For adiabatic premixed models, your input for

Adiabatic Unburnt Temperature (

) will also be used in Equation . in the Theory Guide to calculate

the temperature.

The other properties specified for the unburnt mixture are viscosity, specific heat, thermal conductivity,

and any other properties related to other models that are being used in conjunction with the premixed

combustion model.

For premixed combustion models, you will need to set an additional boundary condition at flow inlets

and exits: the progress variable, . Valid inputs for the Progress Variable are as follows:

: unburnt mixture

: burnt mixture

Often, it is sufficient to initialize the progress variable  to  (burnt) everywhere and allow the unburnt

(

) mixture entering the domain from the inlets to blow the flame back to the stabilizer. A better

initialization is to patch an initial value of  (unburnt) upstream of the flame holder and a value of

(burnt) in the downstream region (after initializing the flow field in the Solution Initialization task

page).

Solution →

The Extended Coherent Flame Model (ECFM) solves a transport equation for the flame surface area

density, denoted , in addition to the reaction progress variable. Details about setting up the reaction

progress variable boundary and initial conditions, and material properties, can be found in Setting Up

the C-Equation and G-Equation Models (p. ). To use the ECFM, select Extended Coherent Flame

Model as the Premixed Model. A list of Extended Coherent Flame Model Constants will appear in

the Species Model dialog box.

... Modifying the ECFM Model Variant

... Modifying the Constants for the ECFM Flame Speed Closure

... Setting Boundary Conditions for the ECFM Transport

... Initializing the Flame Area Density

The source terms for Equation . in the Theory Guide are determined by which ECFM model variant

is used. There are four ECFM model variants available. The default Veynante scheme is the recommended

scheme, because it provides the best accuracy in most situations. If you want access to a different

model variant, you must use the following text command:

define → models → species → set-premixed-combustion

You can then revise the model constants as necessary. See Closure for ECFM Source Terms in the

Theory Guide for further details. If you are using LES turbulence modeling, see LES and ECFM as well.

In the Extended Coherent Flame Model Constants group box of the Species Model dialog box, select

the ITNFS Treatment. You have a choice of constant-delta, meneveau, blint, poinsot, or constant.

The various ITNFS treatments are described in detail in Closure for ECFM Source Terms in the Theory

Guide.

The treatment you select will determine which constants you can set. In all cases, you need to define

the Turbulent Schmidt Number (

) and the Wall Flux Coefficient. If you selected the constant-

delta treatment, you can set the ITNFS Flame Thickness (

in Equation . in the Theory Guide). If

you selected the constant treatment, you can set the ITNFS Value (

Guide). Note that, in general, you will not need to modify the constants available in the Extended

Coherent Flame Model Constants group box because the default values are suitable for a wide range

of premixed flames.

Setting Up the Extended Coherent Flame Model

Figure . : The Species Model Dialog Box for ECFM

For the ECFM transport equation option for the premixed combustion models, you will need to set an

additional boundary condition at flow inlets and exits: the flame area density,

. Valid inputs for the

Flame Area Density are as follows:

: no flame area (unburned)

: burning with nonzero flame area

Often, it is sufficient to initialize the flame area density  to  (laminar flame speed) everywhere and

allow the unburnt mixture entering the domain from the inlets to develop. Another option for initial-

ization is to patch an initial value of  (not burning) upstream of the flame holder and a value of

or higher (burning) in the downstream region (after initializing the flow field in the region).

ANSYS Fluent provides several additional reporting options for premixed combustion calculations. You

can generate graphical plots or alphanumeric reports of the following items:

Adiabatic Flame Temperature

These variables are contained in the Premixed Combustion... category of the variable selection drop-

down list that appears in postprocessing dialog boxes. See Field Function Definitions (p. ) for a

complete list of flow variables, field functions, and their definitions. Displaying Graphics (p. ) and

Note that Static Temperature and Adiabatic Flame Temperature will appear in the Premixed Com-

bustion... category only for adiabatic premixed combustion calculations; for non-adiabatic calculations,

Static Temperature will appear in the Temperature... category. Unburnt Fuel Mass Fraction will appear

only for non-adiabatic models.

ANSYS Fluent also provides several additional reporting options for premixed combustion calculations

with the ECFM model for flame speed closure. You can generate graphical plots or alphanumeric reports

of the same items that are available with the premixed mode, and in addition:

Progress Variable Curvature

These variables will also appear in the Premixed Combustion... category.

ANSYS Fluent also provides two additional reporting options for premixed combustion calculations with

the G-Equation model:

Postprocessing for Premixed Combustion Calculations

The Variance of Distance from Flame is the variance of the distance of the instantaneous flame from

the mean flame position. These variables appear in the Premixed Combustion... category.

... Computing Species Concentrations

If you know the composition of the unburnt and burnt mixtures in your model (that is, if you have

performed separate ANSYS Fluent or external analyses of chemical equilibrium calculations or 1D

premixed flames), you can compute the species concentrations in the domain using custom field

functions:

To determine the concentration of a species in the unburnt mixture, define the custom function

,

where

is the mass fraction for the species in the unburnt mixture (specified by you) and  is the value

of the progress variable (computed by ANSYS Fluent).

To determine the concentration of a species in the burnt mixture, define the custom function

, where

is the mass fraction for the species in the burnt mixture (specified by you) and  is the value of the

progress variable (computed by ANSYS Fluent).

See Custom Field Functions (p. ) for details about defining and using custom field functions.

Chapter : Modeling Partially Premixed Combustion

This chapter describes how to use the ANSYS Fluent's partially-premixed combustion model that is

based on the non-premixed combustion model (Modeling Non-Premixed Combustion (p. )) and the

premixed combustion model (Modeling Premixed Combustion (p. )). For information about the theory

behind the partially premixed combustion model, see Partially Premixed Combustion in the Fluent

Information about using the partially premixed combustion model is presented in the following sections:

.. Limitations

.. Using the Partially Premixed Combustion Model

The underlying theory, assumptions, and limitations of the non-premixed and premixed models apply directly

to the partially premixed model. In particular, the single-mixture-fraction approach is limited to two inlet

streams, which may be pure fuel, pure oxidizer, or a mixture of fuel and oxidizer.The two-mixture-fraction

model extends the number of inlet streams to three, but incurs a major computational overhead. See Limit-

ations of the Premixed Combustion Model (p. ) for additional limitations.

The Flamelet Generated Manifold (FGM) model is limited to the c-Equation partially-premixed model.

The procedure for setting up and solving a partially premixed combustion problem combines parts of

the non-premixed combustion setup and the premixed combustion setup. An outline of the procedure

is provided in Setup and Solution Procedure (p. ), along with information about where to look in the

non-premixed and premixed combustion chapters for details. Inputs that are specific to the partially

premixed combustion model are provided in this chapter.

Information is provided in the following sections:

... Setup and Solution Procedure

... Flamelet Generated Manifold

... Calculating the Look-Up Tables

... Standard Files for Flamelet Generated Manifold Modeling

... Modifying the Unburnt Mixture Property Polynomials

... Setting Premix Flame Propagation Parameters

... Modeling In Cylinder Combustion

... Postprocessing for FGM Scalar Transport Calculations

. Read your mesh file into ANSYS Fluent and set up any other models you plan to use in conjunction with

the partially premixed combustion model (turbulence, radiation, and so on).

. Enable the partially premixed combustion model.

a.

Turn on the Partially Premixed Combustion model in the Species Model dialog box.

Note

Make sure a turbulence model (other than the Spalart-Allmaras model) is selected

before selecting a combustion model.

Edit...

b. If you select the C Equation as the Premixed Model, then you have the choice of selecting one of

the following State Relation models in the Chemistry tab: Chemical Equilibrim, Steady Diffusion

Flamelet, Unsteady Diffusion Flamelet (for steady-state simulations starting from a converged Steady

Diffusion Flamelet solution), or Flamelet Generated Manifold.

c.

If you select the Extended Coherent Flame Model, then you can select Chemical Equilibrim, Steady

Diffusion Flamelet, and Unsteady Diffusion Flamelet.You can modify the Extended Coherent

Flamelet Model Constants in the Premix tab. See Modifying the Constants for the ECFM Flame Speed

Closure (p. ) for details.

Note

Note that the Extended Coherent Flame Model (ECFM) may be deprecated in future

releases.

d. If you select the G Equation as the Premixed Model, then you have the choice of selecting one of

the following State Relation models in the Chemistry tab: Chemical Equilibrim or Steady Diffusion

Flamelet.

. In the Chemistry tab of the Species Model dialog box, select the appropriate State Relation based on

the type of partially premixed model you want to simulate. In ANSYS Fluent, there are two types of partially

premixed models, namely a thin-flamelet model (equilibrium and diffusion flamelet) and a finite-thickness

flamelet model, which is a Flamelet Generated Manifold.You can refer to Non-Premixed Combustion in

the Fluent Theory Guide to learn about diffusion flamelets or Partially Premixed Combustion Theory in the

Fluent Theory Guide for FGMs. Also, you can refer to Overview in the Fluent Theory Guide for general inform-

ation about the thin-flamelet and finite-thickness flamelet models.

. If you select Flamelet Generated Manifold, you will also need to define whether the FGM is calculated

from a premixed or a diffusion flamelet, as well as the Turbulence-Chemistry Interaction in the Premix

tab.The available options (Finite-Rate and Turbulent Flame Speed) are discussed in FGM Turbulent

Closure in the Fluent Theory Guide.

. In the Flamelet tab, you can modify the Flamelet Parameters as described in Flamelet Generated Mani-

fold (p. ).

Modeling Partially Premixed Combustion

. Generate a PDF look-up table.The table parameters are defined in Calculating the Look-Up Tables (p. ).

Important

fold (p. ).

Important

If ANSYS Fluent warns you during the partially premixed properties calculation that any

parameters are out of the range for the laminar flame speed function, you will need to

modify the piecewise-linear points manually before saving the PDF file. See Modifying

the Unburnt Mixture Property Polynomials (p. ) for details. Also, the calculation of the

thermal diffusivity uses the thermal conductivity in the Create/Edit Materials dialog

box. More accurate thermal diffusivity polynomials can be obtained by editing the

thermal conductivity in the Create/Edit Materials dialog box and then clicking Recal-

culate Properties in the Properties tab.

. Define the physical properties for the unburnt material in the domain.

Setup →

Materials

ANSYS Fluent will automatically select the prepdf-polynomial function for Laminar Flame Speed,

indicating that the piecewise-linear polynomial function from the PDF look-up table will be used

to compute the laminar flame speed. You may also choose to enter a constant value, use a user-

defined function, metghalchi-keck-law, or apply laminar-flame-speed-library instead of a

piecewise-linear polynomial function. See Laminar Flame Speed in the Fluent Theory Guide and

Defining Physical Properties for the Unburnt Mixture (p. ) for information about setting the

other properties for the unburnt material.

. Set the values for the mean progress variable ( ) and the mean mixture fraction ( ) and its variance (

)

at flow inlets and exits. (For problems that include a secondary stream, you will define boundary conditions

)

for the mean secondary partial fraction and its variance as well.)

Setup →

See Defining Non-Premixed Boundary Conditions (p. ) for guidelines on setting mixture fraction

and variance conditions, as well as thermal and velocity conditions at inlets.

Important

There are two ways to specify a premixed inlet boundary condition:

a.

If you defined the fuel composition in the Boundary tab to be the premixed inlet species,

then you should set

and

in the boundary condition dialog boxes.

b. If you set the fuel composition to pure fuel in the Boundary tab, you will need to set the

correct equivalence ratio (

) and

at your premixed inlet boundary condition.

For example, if the premixed inlet of methane and air is at an equivalence ratio of ., you can

a.

specify the mass fraction of the fuel composition of

= .,

= ., and

= . in the

Boundary tab and  =  and  =  in the boundary condition dialog box.

Using the Partially Premixed Combustion Model

b. specify the mass fraction of the fuel composition of

= . in the Boundary tab and  = . and

=  in the boundary condition dialog box.

Method (a) is preferred since it will have more points in the flame zone than method (b).

. Initialize the value of the progress variable.

Solution →

See Initializing the Progress Variable (p. ) for details.

. Solve the problem and perform postprocessing.

See Solving the Flow Problem (p. ) for guidelines about setting solution parameters. (These

guidelines are for non-premixed combustion calculations, but they are relevant for partially premixed

as well.)

as well.)

. Click the Import Flamelet File... button. In The Select File Dialog Box (p. ), select the file to be read in

to ANSYS Fluent.

The ANSYS Fluent Flamelet Generated Manifold (FGM) model has several advantages over the thin-

flame equilibrium or diffusion steady flamelet models, such as the ability to model flame quenching

due to dilution. The manifold can be modeled with either a Premixed Flamelet or a Diffusion

Flamelet.

When Premixed Flamelet is selected as the Flamelet Type, you can select to solve the flamelets either

in the Progress Variable Space or in the CHEMKIN Physical Space (Flamelet Solution Method group

box). For more information about these methods, see Premixed FGMs in Reaction Progress Variable

Space and Premixed FGMs in Physical Space in the Fluent Theory Guide.

To generate a flamelet file, go to the Flamelet tab of the Species Model dialog box (Figure . : The

Species Model Dialog Box (Flamelet Tab) (p. )), where you will enter values for parameters of the

flamelet.

.... Premixed Flamelet Generated Manifolds

For premixed Flamelet Generated Manifolds, details about specifying the Scalar Dissipation at Stoi-

chiometric Mixture Fraction can be found in Premixed FGMs in Reaction Progress Variable Space in

Figure . : Premixed Flamelet Generated Manifolds (Flamelet Tab)

The Flamelet Parameters for premixed FGMs are as follows:

Number of Grid Points in Mixture Fraction Space

(

). Increased resolution will provide greater accuracy, but since premixed flamelets are solved at all

mixture fraction points, the flamelet computation time will increase linearly with this input.

Number of Grid Points in Reaction Progress Space

specifies the number of reaction progress grid points distributed between unburnt (

) and burnt

(

) states. Increased resolution will provide greater accuracy. However, when the flamelets are gener-

ated in the Progress Variable Space, the computation time and the required memory for the flamlets

calculation will increase with increasing resolution.

Scalar Dissipation at Stoichiometric Mixture Fraction

specifies the premixed flamelet strain rate.The default of /s is an approximate value of the scalar

dissipation of a freely propagating (unstrained) premixed flame at stoichiometric mixture fraction (unity

equivalence ratio).This option is available only when the premixed FGM is generated in the Progress

Variable Space.

Guide.

has a default of .

has a default of . and is

Refine flamelet based on

allows you to select either the Stoichiometric mixture fraction or Specified mixture fraction. For

Specified mixture fraction, you must also specify a mixture fraction level at which the flamelet is

solved during the grid refinement.

Note

When CHEMKIN Physical Space is selected as the Flamelet Solution Method for the

Premixed Flamelet, the following default values are used for the Automated Grid Refine-

ment parameters:

Initial Number of Grid Points in Flamelet =

Maximum Number of Grid Points in Flamelet =

Maximum Change in Value Ratio = .

Maximum Change in Slope Ratio = .

Click Calculate Flamelets to begin the premixed flamelet calculation.

.... Diffusion Flamelet Generated Manifolds

Generating diffusion Flamelet Generated Manifolds is similar to generating Steady Diffusion Flamelets,

as described in Calculating the Flamelets (p. ).

Figure . : Diffusion Flamelet Generated Manifolds (Flamelet Tab)

The parameters for the diffusion FGM flamelet are slightly different than those for the premixed FGM

flamelet (see Premixed Flamelet Generated Manifolds (p. ) for the definitions of the parameters).

The additional diffusion FGM flamelet parameters are as follows:

Fluent Theory Guide.

specifies the interval between scalar dissipation values (in s-) for which multiple flamelets will be calcu-

lated.This corresponds to

Note

The FGM model does not require the Maximum Number of Flamelets parameter. Instead,

ANSYS Fluent increases the scalar dissipation until the flamelet extinguishes. Hence, the

Scalar Dissipation Step should be set at approximately one twentieth of the counterflow

diffusion flamelet extinction strain rate, so that about twenty flamelets are calculated.The

final, extinguishing unsteady diffusion flamelet is used to model the manifold between

the unburnt state (

) and the last steady diffusion flamelet at the highest scalar dissipation

rate just before extinction.

Scalar Dissipation Multiplier and Scalar Dissipation Step are used to specify the interval

of scalar dissipation for <  and ≥ , respectively. For example, for initial scalar dissipation

of 1e- s- with a Scalar Dissipation Multiplier of , and a Scalar Dissipation Step of ,

the flamelets will be generated with scalar dissipations of 1e-, 1e-, ., ., , , , and

so on.

determines how the progress variable (Equation . in the Fluent Theory Guide) is calculated. If this option

is selected, ANSYS Fluent will compute the progress variable using equilibrium. Otherwise, the progress

variable will be computed using the solution of flamelet generated with initial scalar dissipation as a

denominator in Equation . in the Fluent Theory Guide.

these inputs control the number of discrete values for which the look-up tables will be computed.

These parameters are input in the Table tab of the Species Model dialog box.

For the example of modeling a partially-premixed flame with either the premixed or the diffusion FGM

model, the Table tab of the Species Model dialog box is shown in Figure . : The Species Model

Dialog Box: Table Tab with no Automated Grid Refinement (p. ) when the Automated Grid Refinement

(AGR) is disabled and Figure . : The Species Model Dialog Box: Table Tab Displaying Automated Grid

Refinement (p. ) when the AGR is enabled.

Figure . : The Species Model Dialog Box: Table Tab with no Automated Grid Refinement

When the automated grid refinement is not selected, the look-up table parameters specific to the

partial-premixed model are as follows:

Number of Mean Progress Variable Points

is the number of discrete values of  at which the look-up tables will be computed.This number is de-

termined from the number of grid points in the flamelet.

Number of Progress Variable Variance Points

axis is, in general, not as steep as the variation along the

axis of the look-up tables.

pre-calculated with all the species, and hence the convergence behavior of ANSYS Fluent will not be af-

fected by the input for the Maximum Number of Species. Hence, to keep table sizes small, you should

set the Maximum Number of Species to only include the species that you are interested in postprocessing.

the chemical system that you are considering, with more points required in high heat release systems

(for example, hydrogen/oxygen flames).

is used to determine the lowest temperature for which the look-up tables are generated.Your input

should correspond to the minimum temperature expected in the domain (for example, an inlet or wall

temperature).The minimum temperature should be set – K below the minimum system temperature.

This option is available only if you are modeling a non-adiabatic system.

Figure . : The Species Model Dialog Box: Table Tab Displaying Automated Grid Refinement

The look-up table parameters when Automated Grid Refinement is selected are as follows:

specifies the number of grid points for the resolution of the mean mixture fraction, mixture fraction

variance, and mean enthalpy (for non-adiabatic systems); and mean progress variable and progress variable

variance (for FGM).

specifies the maximum number of grid points used for tabulation.The grid refinement procedure will

stop inserting the points when either the change in value and slope between successive points is within

tolerance or the maximum number of grid points are generated.

Note

Note

For the FGM model, you can solve additional transport equations for selected species mass fractions,

called FGM scalars, as described in Scalar Transport with FGM Closure in the Fluent Theory Guide. To

do so, click FGM Scalar Transport.

Figure . : The Select Transported Scalars Dialog Box

In the Select Transported Scalars dialog box that opens, select the FGM scalars as follows:

To add a species to the Transported Scalars list, select it in the Available Species multiple-selection list

and click Add.

To remove a species from the Transported Scalars list back to the Available Species multiple-selection

list, select it and click Remove.

For flow boundaries, you can specify the boundary conditions for the Scalar Mass Fractions for the

selected transported scalars (in the Species tab of the corresponding boundary conditions dialog

boxes).

During the solution run, ANSYS Fluent will solve transport equations for the selected scalars and take

their pre-computed averaged reaction rates from the PDF look-up table.

Note

You must select the FGM transported scalars before calculating the PDF table. Once the table

is calculated, you will no longer be able to modify the definition of the transported FGM scalars.

In order to modify the FGM scalar definition after the PDF table has been calculated, you will

need to re-import or regenerate the flamelets.

Since the scalar equations do not couple back into the flow equations or mixture properties,

they could be solved in a postprocessing mode for a steady-state simulation, such as pollutant

formation. In such cases, you could deselect FGM Scalar Transport from the Equations list

solved by ANSYS Fluent (in the Equations dialog box), and then select them again once the

steady flow field has converged.

.... Postprocessing the Look-Up Tables with Flamelet Generated Manifolds

For the FGM model, the PDF table is four-dimensional for adiabatic cases and five-dimensional for

non-adiabatic cases. For adiabatic PDF tables, the four independent variables are Mean mixture fraction,

Mean reaction progress variable, Mixture fraction variance, and Progress variable variance. For non-

adiabatic tables, the additional fifth independent variable is enthalpy. The FGM PDF tables can be

post-processed using 2D curves and 3D surfaces by fixing two or more independent variables.

The procedure to display the lookup tables graphically is similar to that outlined in Postprocessing

the Look-Up Table Data (p. ) with additional steps as follows.

Adiabatic PDF Tables

Figure . : The PDF Table Dialog Box (Adiabatic Case With FGM)

– 3D surfaces:

. Under Volume Parameters, select the discrete independent parameter to be held constant and fix

it by specifying either a slice Index number or a Value. (For more information, see Postprocessing

the Look-Up Table Data (p. ).)

. In a similar manner, under Surface Parameters, select and fix the second discrete independent

parameter and click Plot.

The resulting plot is a 3D surface of the selected Plot Variable as a function of the remaining

two independent variables that have not been fixed.

– 2D curves on 3D Surface:

. Under Volume Parameters and Surface Parameters, fix discrete independent parameters as de-

scribed above.

. Under the Curve Parameters group box, select the X-Axis Function against which the plot variable

will be displayed, fix the remaining discrete independent parameter using controls in the Constant

Value of Independent Parameter  group box, and click Plot.

The resulting plot is a 2D curve of the selected Plot Variable  as a function of the remaining

independent variable that has not been fixed.

Non-Adiabatic PDF Tables

Figure . : The PDF Table Dialog Box (Non-Adiabatic Case With FGM)

. Fix the enthalpy slice level by specifying Enthalpy Slice.

For non-adiabatic PDF tables, heat loss/gain is the fifth independent variable, which is expressed

as enthalpy levels. By default, the enthalpy level is fixed at the adiabatic level, which is displayed

in the Enthalpy Slice, Adiabatic = slice number  label, as shown in Figure . : The PDF

Table Dialog Box (Non-Adiabatic Case With FGM) (p. ). Enthalpy slice numbers below the

adiabatic slice number are associated with heat loss, while enthalpy slice numbers above the

adiabatic slice number are associated with enthalpy gain.

. Depending on whether you want to display a 3D surface or a 2D Curve on 3D Surface, follow appropriate

steps for Adiabatic PDF Tables described above.

A standard flamelet file format can be used to read and write FGM flamelets. The data structure for

the standard flamelet file format is based on keywords that precede each data section. If any of the

keywords in your flamelet data file do not match the supported keywords, you will have to manually

edit the file and change the keywords to one of the supported types. (The ANSYS Fluent flamelet filter

is case-insensitive, so you need not worry about capitalization within the keywords.)

Header section: HEADER

Main body section: BODY

Number of species: NUMOFSPECIES

Number of grid points: GRIDPOINTS

Pressure: PRESSURE

Temperature: TEMPERATURE and TEMP

Mass fraction: MASSFRACTION-

Mixture fraction: Z

Mole fraction: MOLEFRACTION-

Scalar dissipation for premixed flamelet: PREMIX_CHI

Reaction progress: REACTION_PROGRESS

Reaction progress source term: PREMIX_YCDOT

Note

Note that the FGM standard flamelet file format is identical for both premixed and diffusion

flamelets. However, this format is different from the standard format for steady diffusion

Laminar Flamelets, which is described in Calculating the Look-Up Tables (p. ).

.... Sample Standard FGM File

A sample FGM file in the standard FGM format is provided below. Note that not all species are listed

in this file.

HEADER

PREMIX_STOICH_SCADIS   .000000E+

Z         .000000E+

STOICH_Z    .520020e-

PRESSURE  .013250E+

BODY

REACTION_PROGRESS

.000000000E+   .625000000E-   .125000000E-   .687500000E-   .250000000E-

BODY

.812500000E-   .375000000E-   .937500000E-   .500000000E-   .062500000E-

.625000000E-   .187500000E-   .750000000E-   .312500000E-   .875000000E-

.437500000E-   .000000000E-   .508132748E-   .604275079E-   .668740305E-

.718608224E-   .759835686E-   .795270729E-   .826516818E-   .854574013E-

.880111737E-   .903602004E-   .925391181E-   .945741609E-   .964857158E-

.982899681E-   .000000000E+

.000000000E+   .000000063E+   .000000126E+   .000000189E+   .000000251E+

.000000314E+   .000000377E+   .000000440E+   .000000503E+   .000000566E+

.000000628E+   .000000691E+   .000000754E+   .000000817E+   .000000880E+

.000000943E+   .000001006E+   .000001062E+   .000001073E+   .000001080E+

.000001086E+   .000001090E+   .000001094E+   .000001098E+   .000001101E+

.000001104E+   .000001107E+   .000001109E+   .000001111E+   .000001113E+

.000001115E+   .000001117E+

massfraction-h2

.000000000E+   .095241207E-   .190482414E-   .285723620E-   .380964827E-

.476206034E-   .571447241E-   .666688448E-   .761929655E-   .857170861E-

.095241207E-   .204765328E-   .314289448E-   .423813569E-   .533337690E-

.642861810E-   .752385931E-   .851324229E-   .870044058E-   .882596053E-

.892305813E-   .900333194E-   .907232735E-   .913316647E-   .918779651E-

.923752089E-   .928325868E-   .932568429E-   .936530852E-   .940252832E-

.943765883E-   .947095479E-

. . . . .

. . . . .

PREMIX_YCDOT

.000000000E+   .000000000E+   .000000000E+   .000000000E+   .000000000E+

. . . . .

. . . . .

.000000000E+   .000000000E+

After building the PDF table, ANSYS Fluent automatically calculates the temperature, density, heat

capacity, and thermal diffusivity of the unburnt mixture as polynomial functions of the mean mixture

fraction,

(see Equation . in the Fluent Theory Guide). The laminar flame speed is automatically

calculated as a piecewise-linear polynomial function of .

However, as outlined in Partially Premixed Combustion Theory in the Fluent Theory Guide, the laminar

flame speed depends on details of the chemical kinetics and molecular transport properties, and in

the prepdf-polynomial method, it is not calculated directly. Instead, curve fits are made to flame speeds

determined from detailed simulations  [] (p. ). These fits are limited to a range of fuels (H2, CH4,

C2H2, C2H4, C2H6, and C3H8), air as the oxidizer, equivalence ratios of the lean limit through unity, unburnt

temperatures from  K to  K, and pressures from  bar to  bars. If your parameters fall outside

this range, ANSYS Fluent will warn you when it computes the look-up table. In this case, you will need

to modify the piecewise-linear points in the Properties tab of the Species Model dialog box (Fig-

ure . : The Species Model Dialog Box (Properties Tab) (p. )) before you save the PDF file. If you

selected the laminar-flame-speed-library method, ANSYS Fluent will report the computed laminar

flame speed. Note that the table values cannot be modified.

Figure . : The Species Model Dialog Box (Properties Tab)

For each polynomial function of  under Partially Premixed Mixture Properties (Adiabatic Unburnt

Density, Adiabatic Unburnt Temperature, Unburnt Cp, and Unburnt Thermal Diffusivity), you can

specify values for Coefficient , Coefficient , Coefficient , and Coefficient  (the polynomial coef-

ficients in Equation . in the Fluent Theory Guide) in the appropriate Quadratic of Mixture Fraction

dialog box (Figure . : The Quadratic of Mixture Fraction Dialog Box (p. )). To open this dialog box,

click the appropriate Edit... button in the Properties tab.

Figure . : The Quadratic of Mixture Fraction Dialog Box

If you selected the prepdf-polynomial method, you can also specify the piecewise-linear Mixture

Fraction and its corresponding Laminar Flame Speed for  different points in the Piecewise Linear

dialog box (Figure . : The Piecewise Linear Dialog Box (p. )). The first set of values is the lower

limit and the last set of values is the upper limit. Outside of either limit, the laminar flame speed is

constant and equal to that limit. If you selected the laminar-flame-speed-library method, you can display

the table, but you cannot modify the table values. To open the Piecewise Linear dialog box, click the

Edit... button next to Laminar Flame Speed in the Properties tab.

Figure . : The Piecewise Linear Dialog Box

Important

Note also that if you choose to use a user-defined function for the laminar flame speed in

the Create/Edit Materials Dialog Box (p. ), the piecewise-linear fit becomes irrelevant.

If the secondary mixture fraction model is enabled, the unburnt properties are a function of both the

mean and secondary mixture fractions. An additional column is added in the Piecewise Linear dialog

box for the secondary mixture fraction unburnt polynomial coefficients.

Note that the Non-Adiabatic Laminar Flame Speed option when enabled includes the non-adiabatic

effects on the laminar flame speed by tabulating the laminar speeds in the PDF table. See Laminar

Flame Speed in the Fluent Theory Guide.

Once the PDF look-up table is generated, you can specify the turbulent flame speed model options

in the Premixed tab of the Species Model dialog box. For the FGM model, you can also specify the

variance settings and select the turbulence-chemistry interaction model.

Figure . : The Species Model Dialog Box(Premix Tab)

The following controls are available in the Turbulent Flamelet Speed Model group box.

Flame speed Model

allows you to select the method to calculate turbulent flame speed as described in Turbulent Flame Speed

Models in the Fluent Theory Guide.

If you selected zimont, you can adjust the Zimont model parameters as described in Modifying

the Constants for the Zimont Flame Speed Model (p. ).

When the SBES turbulence model is used with the C Equation premixed model, you can also specify

the following additional inputs:

Turbulent Length Scale Constant (RANS)

is the modeling constant in the RANS region (

Turbulent Flame Speed Constant (RANS)

is the modeling constant in the RANS region (  in Equation . in the Theory Guide).

If you selected peters, you can adjust the Peters model parameters as described in Modifying the

Constants for the Peters Flame Speed Model (p. ).

For the FGM model, you can adjust the following additional parameters:

Turbulence-Chemistry Interaction

allows you to choose the method for modeling the source term in the progress variable equation (Equa-

tion . in the Fluent Theory Guide).The following methods are available:

Finite-Rate: Uses Equation . in the Fluent Theory Guide to calculate progress variable source terms

from the PDF table.

Turbulent Flame Speed: Uses Equation . in the Fluent Theory Guide to calculate progress variable

reaction source terms.

For more information about these models, see FGM Turbulent Closure in the Theory Guide.

Variance Settings

contains the Variance Method drop-down list that allows you to choose between the following methods

for calculating the progress variable variance:

transport equation (Equation . in the Fluent Theory Guide)

algebraic (Equation . in the Fluent Theory Guide)

(SBES only) hybrid  (Equation . in the Fluent Theory Guide)

For the hybrid  option, when applying Equation . in the Fluent Theory Guide, the algebraic

model is used for

and the transport equation model is used for

.

For the algebraic and hybrid  options, you need to specify Algebraic Variance Constant (

in

Equation . in the Fluent Theory Guide).

It is recommended that you use the transport equation option for RANS, the algebraic option

for LES, and the hybrid  option for SBES.

Each of the partially premixed combustion models may be used for modeling in cylinder combustion.

When modeling more than one cycle of such engines, you may choose to model trapped combustion

products and exhaust gas recirculation (EGR) using the inert species model (see Setting Up the Inert

Model (p. )). A Dynamic Mesh Event has also been provided for calculating the inert composition,

converting burned gases to inert and resetting the combustion process ready for the next cycle (see

Resetting Inert EGR (p. ) and Resetting Inert EGR (p. )).

In the case of the G-Equation model, this is the only way to automatically model multiple in cylinder

combustion cycles and take into account trapped burned gases remaining in the cylinder from one

cycle to the next.

ANSYS Fluent provides additional reporting options when you use the FGM Scalar Transport option

for solving transport equations for the FGM scalars selected in the Select Transported Scalars dialog

box. Quantities for reporting scalar mass fractions of the FGM scalars are contained in the Premixed

Combustion… category the postprocessing dialog boxes.

Chapter : Modeling a Composition PDF Transport Problem

This chapter discusses how to use the composition PDF transport model for modeling finite-rate

chemistry in turbulent flames in ANSYS Fluent. ANSYS Fluent has two different discretizations of the

composition PDF transport equation, namely Lagrangian and Eulerian. The Lagrangian method is more

accurate than the Eulerian method, but requires significantly longer run time to converge. For information

about the theory behind the composition PDF transport model, see Composition PDF Transport in the

Information about using this model is presented in the following sections:

.. Limitation

.. Steps for Using the Composition PDF Transport Model

.. Enabling the Lagrangian Composition PDF Transport Model

.. Enabling the Eulerian Composition PDF Transport Model

.. Initializing the Solution

.. Monitoring the Solution

.. Postprocessing for Lagrangian PDF Transport Calculations

.. Postprocessing for Eulerian PDF Transport Calculations

A limitation that applies to the composition PDF transport model is that you must use the pressure-

based solver as the model is not available with the density-based solver.

The procedure for setting up and solving a composition PDF transport problem is outlined below, and

then described in detail. Remember that only steps that are pertinent to composition PDF transport

modeling are shown here. For information about inputs related to other models that you are using in

conjunction with the composition PDF transport model, see the appropriate sections for those models.

. Read a CHEMKIN-formatted gas-phase mechanism file and the associated thermodynamic data file in the

CHEMKIN Mechanism dialog box (see Importing a Volumetric Kinetic Mechanism in CHEMKIN

Important

If your chemical mechanism is not in CHEMKIN format, you will have to enter the mech-

anism into ANSYS Fluent as described in Overview of User Inputs for Modeling Species

Transport and Reactions (p. ).

. Enable a turbulence model.

Edit...

. Enable the Composition PDF Transport model and set the related parameters. Refer to Enabling the

Lagrangian Composition PDF Transport Model (p. ) and Enabling the Eulerian Composition PDF Transport

Model (p. ) for further details.

Edit...

. Check the material properties in the Create/Edit Materials dialog box and the reaction parameters in the

Reactions dialog box.The default settings should be sufficient.

Setup →

Materials

. Set the operating conditions, cell zone conditions, and boundary conditions.

Setup →

Setup →

. Check the solver settings.

Solution →

Methods

Solution →

Controls

The default settings should be sufficient, although you should change the discretization to second-

order once the solution has converged.

. Initialize the solution.You may need to patch a high-temperature region to ignite the flame.

Solution →

Initialization → Initialize

Solution →

. Run the solution.

Solution →

Important

Solution →

Solution →

Solution →

Important

A good initial condition can reduce the solution time substantially. You should start from an

existing solution calculated using the Laminar Finite-Rate, EDC model, non-premixed com-

bustion model, or partially premixed combustion model. See   Modeling Species Transport

and Finite-Rate Chemistry (p. ), Modeling Non-Premixed Combustion (p. ), and Modeling

Partially Premixed Combustion (p. ) for further information on such simulations.

Modeling a Composition PDF Transport Problem

To enable the composition PDF transport model, select Composition PDF Transport in the Species

Model dialog box (Figure . : The Species Model Dialog Box for Lagrangian Composition PDF Trans-

port (p. )).

Edit...

When you enable Composition PDF Transport, the dialog box will expand to show the relevant inputs.

. Select Lagrangian under PDF Transport Options.

Figure . : The Species Model Dialog Box for Lagrangian Composition PDF Transport

. Enable Volumetric under Reactions.

Enabling the Lagrangian Composition PDF Transport Model

The Composition Pdf Transport model uses ANSYS Fluent stiff chemistry solver with ISAT enabled

by default. See Using ISAT (p. ) for more details.

. Click the Integration Parameters... button to open the Integration Parameters Dialog Box (p. ) (Fig-

ure . :The Integration Parameters Dialog Box (p. )). For additional information, see Using ISAT (p. ).

Figure . : The Integration Parameters Dialog Box

. Enable Liquid Micro-Mixing to interpolate

from turbulence models and scalar spectra, as noted in Liquid

Reactions in the Theory Guide.This is applied to cases where reactions in liquids occur at low turbulence

levels, among reactants with low diffusivities.Therefore, a default value of

may not be desirable, as

it over-estimates the mixing rate.

. In the Mixing tab, select Modified Curl, IEM, or EMST under Mixing Model and specify the value of the

Mixing Constant (

in Equation . in the Theory Guide). For more information about particle diffusion,

see Particle Mixing in the Theory Guide.

Important

If the Liquid Micro-Mixing option is enabled, you cannot set the Mixing Constant.

. You will not be specifying species boundary conditions in the Boundary tab.This is only applicable to the

Eulerian PDF Transport Option.

. In the Control tab, you will specify the Lagrangian PDF transport control parameters.

Particles Per Cell

sets the number of PDF particles per cell. Higher values of this parameter will reduce statistical error,

but increase computational time.

Local Time Stepping

is available for steady-state simulations and can increase the convergence rate by taking maximum

allowable time-steps on a cell-by-cell basis. (see Equation . of the Theory Guide). If Local Time

Stepping is enabled, then you can specify the following parameters:

Convection #

specifies the particle convection number (see

Diffusion #

specifies the particle diffusion number (see

Mixing #

Mixing #

specifies the particle mixing number (see

Edit...

. Select Eulerian under PDF Transport Options.

Enabling the Eulerian Composition PDF Transport Model

Figure . : The Species Model Dialog Box for Eulerian Composition PDF Transport

. Enable Volumetric under Reactions.The Stiff Chemistry Solver is disabled by default and should be

enabled if the kinetic mechanism is numerically stiff.

ure . :The Integration Parameters Dialog Box (p. )). See Using ISAT (p. ) for detailed information

about this dialog box.

. Enable Inlet Diffusion to include the diffusive transport of species through the inlets of your domain.

Disable this option if the convective flux at one of the inlets is very small, resulting in mass loss by diffusion

through that inlet.

. Make sure that Diffusion Energy Source is enabled if you want to include species diffusion effects in the

energy equation.

. Enable Liquid Micro-Mixing if the fuel and oxidizer are liquids with low diffusivities (high Schmidt numbers).

In this case, the Mixing Constant will be calculated according to Equation . in the Theory Guide.

. By default, the Laminar (one mode) energy equation is solved, where temperature fluctuations are ignored.

By enabling Include Temperature Fluctuations, the multi-mode energy equation will be solved as done

for species.

. In the Mixing tab, only the IEM mixing model is available for Eulerian PDF transport.

a.

Specify the value of the Mixing Constant.The default value is  for gas phase species.

Important

b. Enter the number of Flow Iterations per Chemistry Update.This is the frequency at which ANSYS

Fluent will update the chemistry during the calculation. Increasing the number can reduce the compu-

tational expense of the chemistry calculations.

c.

Enter the Aggressiveness Factor.This is a numerical factor that controls the robustness and the con-

vergence speed.This value ranges between  and , where  is the most robust, but results in the

slowest convergence.The default value for the Aggressiveness Factor is ..

. In the Boundary tab, define the compositions of the fuel and oxidizer.You can select the boundary species

to be displayed as described in Overview of the Problem Setup Procedure (p. ).

. (Eulerian PDF Transport only) Optionally, you can select the monitored species as described in Overview

of the Problem Setup Procedure (p. ).

... Defining Species Boundary Conditions

At flow inlets, specify the Mixture Fraction in the Species tab of the boundary condition inlet dialog

boxes, as shown in Figure . : The Velocity Inlet Dialog Box for Eulerian Composition PDF Trans-

port (p. ). At outlet boundaries, similarly specify the Backflow Mixture Fraction. ANSYS Fluent always

applies zero flux boundary conditions at walls for all species.

Figure . : The Velocity Inlet Dialog Box for Eulerian Composition PDF Transport

.... Equilibrating Inlet Streams

The Equilibrate Inlet Stream option in the Species tab of the boundary conditions dialog boxes will

set the inlet compositions to their chemical equilibrium values. This option can be used to model

pilot flames  and exhaust gas recirculation.

Important

This option should not be enabled for pure fuel or oxidizer inlets.

If you are using the Eulerian PDF transport model, specify the discretization and under-relaxation for

the Eulerian PDF composition transport in the Solution Controls and Solution Methods task page.

For the Eulerian PDF Transport model, the initialization variables are the mixture fraction and the tem-

perature. The species mass fractions and enthalpy are calculated based on the fuel and oxidizer com-

position (specified in the Species dialog box) and the initialized mixture fraction and temperature.

Figure . : The Solution Initialization Task Page for Eulerian Composition PDF Transport

At low speeds, combustion couples to the fluid flow through density. The Lagrangian PDF transport

algorithm has random fluctuations in the density field, which in turn causes fluctuations in the flow

field. For steady-state flows, statistical fluctuations are decreased by averaging over a number of previous

iterations in the Run Calculation task page (Figure . : The Run Calculation Task Page for Composition

PDF Transport (p. )).

Monitoring the Solution

Figure . : The Run Calculation Task Page for Composition PDF Transport

Averaging reduces statistical fluctuations and stabilizes the solution. However, ANSYS Fluent often in-

dicates convergence of the flow field before the composition fields (temperatures and species) are

converged. You should lower the default convergence criteria in the Residual Monitors Dialog Box (p. ),

and always check that the Total Heat Transfer Rate in the Flux Reports Dialog Box (p. ) is balanced.

It is also recommended that you monitor temperature/species on outlet boundaries and ensure that

these are steady.

The Lagrangian PDF method has the following additional solution controls: Iterations in Average and

Iteration Increment. By increasing the Iterations in Average, fluctuations are smoothed out and resid-

uals level off at smaller values. However, the composition PDF method requires a larger number of iter-

ations to reach steady-state. It is recommended that you use the default of  Iterations in Average

until the steady-state solution is obtained. Then, to gradually decrease the residuals, increase the Itera-

tions in Average by setting a Iteration Increment to a value from  to  (the value . is recommended).

Subsequent iterations will increase the Iterations in Average by the Iteration Increment.

... Running Unsteady Composition PDF Transport Simulations

... Running Compressible Lagrangian PDF Transport Simulations

... Running Lagrangian PDF Transport Simulations with Conjugate Heat Transfer

For unsteady Lagrangian composition PDF transport simulations, a fractional step scheme is employed

where the PDF particles are advanced over the time step, and then the flow is advanced over the time

step. Unlike steady-state simulations, composition statistics are not averaged over iterations, and to

reduce statistical error you should increase the number of particles per cell in the Solution Monitors

For low speed flows, the thermo-chemistry couples to the flow through density. Statistical errors in

the calculation of density may cause convergence difficulties between time step iterations. If you ex-

perience this, increase the number of PDF particles per cell, or decrease the density under-relaxation.

Compressibility is included when ideal-gas is selected as the density method in the Create/Edit Mater-

ials Dialog Box (p. ). For such flows, particle internal energy is increased by

over the time step

, where  is the cell pressure and

is the change in the particle specific volume over the time

step.

step.

... Running Lagrangian PDF Transport Simulations with Conjugate Heat

Transfer

When solid zones are present in the simulation, ANSYS Fluent solves the energy equation in the turbu-

lent flow zones by the Lagrangian Monte Carlo particle method, and the energy equation in the solid

zones by the finite-volume method.

... Reporting Options

... Particle Tracking Options

ANSYS Fluent provides several reporting options for the Lagrangian composition PDF transport calcu-

lations. You can generate graphical plots or alphanumeric reports of the following items:

Mean species-n Mass Fraction

Postprocessing for Lagrangian PDF Transport Calculations

RMS species-n Mass Fraction

The instantaneous composition (Static Temperature and Mass fraction of species-n) in a cell are

calculated as,

(.)

where

= instantaneous cell species mass fraction or temperature at the present

iteration

= number of particles in the cell

= particle mass fraction or temperature

= particle mass

Mean and root-mean-square-error (RMSE) temperatures are calculated in ANSYS Fluent by averaging

instantaneous temperatures over a user-specified number of previous iterations (see Monitoring the

Solution (p. )).

Note that for steady-state simulations, instantaneous temperatures and species represent a Monte

Carlo realization and are as such unphysical. Mean and RMSE quantities are much more useful.

When you have enabled the Lagrangian composition PDF transport model, you can display the traject-

ories of the PDF particles using the Particle Tracks Dialog Box (p. ) (Figure . : The Particle Tracks

Dialog Box for Tracking PDF Particles (p. )).

Results → Graphics → Particle Tracks

New...

Figure . : The Particle Tracks Dialog Box for Tracking PDF Particles

Select the Track PDF Transport Particles option to enable PDF particle tracking. To speed up the

plotting process, you can specify a value  for Skip, which will plot only every

th particle. For details

about setting other parameters in the Particle Tracks dialog box, see Displaying of Trajectories (p. ).

When you have finished setting parameters, click Display to display the particle trajectories in the

To postprocess the Eulerian composition PDF transport model, the following variables are available

for each mode:

Postprocessing for Eulerian PDF Transport Calculations

Mass fraction of species in mode n

Temperature of mode n

Sensible Enthalpy of mode n

Chapter : Using Chemistry Acceleration

ANSYS Fluent can model detailed chemical kinetics in laminar and turbulent flames. Laminar flames are

modeled with the Finite-Rate/No TCI option, while four turbulence-chemistry interaction models are

available for turbulent flames (Finite-Rate/No TCI, Eddy-Dissipation Concept, Lagrangian PDF

Transport, and Eulerian PDF Transport). Detailed chemical mechanisms are invariably numerically stiff

and compute-intensive. ANSYS Fluent provides following methods to accelerate these computations:

ISAT

Dynamic Mechanism Reduction (DMR)

Chemistry Agglomeration

Dimension Reduction

Dynamic Cell Clustering (DCC) (available with the ANSYS CHEMKIN-CFD solver only)

Dynamic Adaptive Chemistry (DAC) (available with the ANSYS CHEMKIN-CFD solver only)

All of the methods are enabled or disabled in the Integration Parameters dialog box, accessed from

the Species Model dialog box by clicking the Integration Parameters... button in the Reactions group

box:

Edit...

All of the acceleration methods induce some accuracy loss, and the controlling parameters should be

carefully adjusted to ensure that this inaccuracy is acceptable, see Chemistry Acceleration in the Fluent

Theory Guide. In most cases, applying ISAT and Dynamic Mechanism Reduction (DMR) together should

give the best performance. Further information about using the chemistry acceleration models is

.. Using ISAT

.. Using Dynamic Mechanism Reduction

.. Using Chemistry Agglomeration

.. Dimension Reduction

.. Using Dynamic Cell Clustering

.. Using Dynamic Adaptive Chemistry with ANSYS Fluent CHEMKIN-CFD Solver

In-Situ Adaptive Tabulation (ISAT) is a storage-retrieval method that constructs a chemistry table at run

time (in-situ) with a user-specified interpolation accuracy (adaptive tabulation). ISAT can be used with

all Chemistry solvers except the None - Explicit Source solver option. ISAT is not available for simulations

with surface reactions.

For ODE solvers (Stiff Chemistry and CHEMKIN-CFD), ANSYS Fluent uses two error tolerances (under

ODE Parameters):

Absolute Error Tolerance: by default, set to -.

Relative Error Tolerance: by default, set to - for the Stiff Chemistry solver and - for the CHEMKIN-CFD

solver.

The default values should be sufficient for most applications, although these tolerances may need to

be decreased for some cases such as ignition. For problems in which the accuracy of the chemistry in-

tegrations is crucial, it may be useful to test the accuracy of the error tolerances in simple zero-dimen-

sional and one-dimensional test simulations with parameters comparable to those in the full simulation.

If you want to use chemistry agglomeration together with ISAT, enable Chemistry Agglomeration in

the Integration Parameters dialog box and specify the chemistry agglomeration Error Tolerance (

).

More information can be found in Using Chemistry Agglomeration (p. ).

... ISAT Parameters

... Monitoring ISAT

... Using ISAT Efficiently

... Reading and Writing ISAT Tables

If you have selected ISAT under Integration Method, you will then be able to set additional ISAT

parameters. The numerical error in the ISAT table is controlled by the ISAT Error Tolerance under

ISAT Parameters. The default ISAT Error Tolerance of . may be sufficiently accurate for temper-

ature and major species, but will most likely need to be decreased to get accurate minor species and

pollutant predictions. For steady-state simulations, it may help to start with a high error tolerance

Using Chemistry Acceleration

during the initial iterations towards a converged solution. A larger error tolerance results in smaller

tables and quicker run times, but greater error.

Important

After your steady simulation is converged, you should always decrease the ISAT Error Tol-

erance and perform further iterations until the species that you are interested in are un-

changed.

The Max. Storage is the maximum RAM used by the ISAT table, and has a default value of  MB.

Generally, you do not need to set it to a value larger than  MB. The value of Verbosity allows you

to monitor ISAT performance in different levels of detail. See Monitoring ISAT (p. ) for details about

this parameter.

To purge the ISAT table, click the Clear ISAT Table button. See Using ISAT Efficiently (p. ) for more

details.

You can monitor ISAT performance by setting the Verbosity in the Integration Parameters dialog

box. For a Verbosity of  or , ANSYS Fluent writes the following information periodically to a file

named case_file_name_stats.out:

total number of queries

total number of queries resulting in retrieves

total number of queries resulting in grows

total number of queries resulting in adds

total number of queries resulting in direct integrations

cumulative CPU seconds in ISAT

cumulative CPU seconds outside ISAT

cumulative wall-clock time in seconds (that is, total CPU time in ISAT plus total CPU time out of ISAT plus

CPU idle time)

The ISAT Verbosity option of  is for expert users who are familiar with ISAT v5. [] (p. ). ANSYS

Fluent writes out the following files for Verbosity = :

table_name_stats.out, as described above

table_name_ODE_accuracy.out reports the accuracy of the ODE integrations. For every new ISAT table

entry, if the maximum absolute error in temperature or species is greater than any previous error, a line is

written to this file.This line consists of the total number of ODE integrations performed up to this time,

the maximum absolute species error, the absolute temperature error, the initial temperature and the time

step.

table_name_ODE_diagnostic.out prints diagnostics from the ODE solver

table_name_ODE_warning.out prints warnings from the ODE solver

Using ISAT

Initially, the table name is equal by default to the current case name, and is changed as the table is

written or read.

Each processor builds its own ISAT table. If Verbosity is enabled, each compute node writes out the

Verbosity file(s) with the node ID number appended to the file name.

Efficient use of ISAT requires thoughtful control. What follows are some detailed recommendations

concerning the achievement of this goal.

Important

The numerical error in the ISAT table is controlled by the ISAT Error Tolerance, which has a

Important

default value of ..This value is relatively large, which allows faster convergence times for

steady-state simulations. However, once the solution has converged, it is important to reduce

this ISAT Error Tolerance and re-converge.This process should be repeated until the species

that you are interested in modeling are unchanged. Unsteady simulations should be run with

a sufficiently small ISAT Error Tolerance so that the species of interest are unaffected by this

parameter. Note that as the error tolerance is decreased, the memory and time requirements

to build the ISAT table will increase substantially.There is a large performance penalty in spe-

cifying an error tolerance smaller than is needed to achieve acceptable accuracy, and the error

tolerance should be decreased gradually and judiciously.

As described in Mesh Partitioning and Load Balancing (p. ), you can select portions of the

simulation to consider when performing dynamic load balancing in multiprocessor simulations.

If the ISAT option is selected in the Weighting tab of the Partitioning and Load Balancing Dialog

Box (p. ), the time required for solving chemistry will be factored in when assigning the

computational cells to each available processor. It is recommended that you select this option

when solving stiff chemistry, particularly when the Dynamic Mechanism Reduction method is

enabled; thus, more resources can be allocated for the cells with the larger mechanisms.

During the initial iterations, before a steady-state solution is attained, transient composition states

occur that are not present in the steady-state solution. For example, you might patch a high temper-

ature region in a cold fuel-air mixing zone to ignite the flame, whereas the converged solution never

has hot reactants without products. Since all states that are realized in the simulation are tabulated

in ISAT, these initial mappings are wasteful of memory, and can degrade ISAT performance. If the table

fills the allocated memory and contains entries from an initial transient that are no longer accessed,

it may be beneficial to purge the ISAT table. This is achieved by either clearing it in the Integration

Parameters dialog box, or saving your case and data files, exiting ANSYS Fluent, then restarting ANSYS

Fluent and reading in the case and data. This can also be done with the TUI command

define/models/species/clear-isat-table.

From experience, ISAT performs very well on premixed turbulent flames, where the range of compos-

ition states are smaller than in non-premixed flames. ISAT performance degrades in flames with large

residence times, where more work is required in the ODE integrator.

ANSYS Fluent can write and subsequently read ISAT tables. However, it is in general not recommended

to write and read ISAT tables for the following reason: ISAT tabulates chemical states that are specific

to a single simulation. The ISAT tabulated composition states are determined by the geometry,

boundary conditions, physics models such as turbulence and radiation, thermodynamic and transport

properties, as well the chemical mechanism. If any of these parameters change, the realized composition

space changes, and significant parts of the existing ISAT table are no longer accessed. These un-accessed

ISAT table entries slow interpolation and decrease the number of useful accessed table entries that

can be added. Since the time consumed building the ISAT table is typically much smaller than simulation

run times, it is advised to rebuild the table when restarting.

When ANSYS Fluent is run in parallel, each partition builds its own ISAT table and does not exchange

information with ISAT tables on other compute nodes. You can save the ISAT tables on all compute

nodes:

File → Write → ISAT Table...

Each compute node writes out its ISAT table to the specified file name, with the node ID number ap-

pended to the file name. For example, a specified file name of my_name on a two compute node run

will write two files called my_name-.isat and my_name-.isat.

Subsequent runs can start from existing ISAT tables by reading them into memory.

File → Read → ISAT Table...

Files can be read in two ways:

Parallel nodes can read in corresponding ISAT tables saved from a previous parallel simulation.The appended

node ID should not be removed from the input file name.

Note

The ability to use ISAT tables generated from a parallel simulation with a different number

of parallel nodes is not supported.

All nodes can read one unique ISAT table.You might use this approach if you have a large table from a

serial simulation. ANSYS Fluent first checks to see if the exact file name that you specified exists, and if it

does, all nodes will read this one file.

Computational time increases with the size of the chemical kinetics mechanism used in the simulation.

Dynamic Mechanism Reduction (DMR) decreases the mechanism size at each cell (or particle) to include

only those species and reactions necessary for accurate modeling (within defined tolerances) of the

chemical kinetics at the local conditions. This is performed at every flow iteration (for steady simulations)

or time step (for transient simulations). Because the mechanism is only required to be accurate at the

local conditions, smaller reduced mechanisms can be used with less accuracy loss than when using

skeletal mechanism reduction, where a single reduced mechanism is used throughout the simulation.

The speed-up from this approach is problem-dependent, but on average is about a factor of two or

more compared to a case with no chemistry acceleration.

For an even greater increase in performance, you can use Dynamic Mechanism Reduction with any

combination of the other chemistry acceleration options available in ANSYS Fluent. In most cases, ap-

plying ISAT and DMR together should give the best performance. Note, however, that ISAT performance

Using Dynamic Mechanism Reduction

degrades when accuracy requirements are very strict or when conditions are not revisited often in a

simulation. An example is unsteady ignition simulations, where ISAT table entries may not be re-used.

However, the important species and reactions can vary widely during the simulation; for example, many

of the low temperature ignition reactions are only required for the small spark zone and short spark

duration. In such situations, you may achieve better performance using Dynamic Mechanism Reduction

along with direct integration method rather than ISAT.

Combining multiple chemistry acceleration methods, however, compounds accuracy loss, since each

of these methods accelerates the simulation by sacrificing some accuracy. In general, greater speed-up

is achievable when the full mechanism is larger, because there is potential for a greater degree of re-

duction.

Important

When using Dynamic Mechanism Reduction along with ISAT, setting the error tolerance for

either approach above its default value degrades accuracy faster than when either method

is used alone.

Dynamic Mechanism Reduction is performed using the Directed Relation Graph (DRG) algorithm. For

details of the DMR algorithm, refer to the discussion in Dynamic Mechanism Reduction in the Fluent

You can enable Dynamic Mechanism Reduction through either the graphical user interface (GUI) or the

text user interface (TUI) as follows.

In the GUI, enable the Dynamic Mechanism Reduction option in the Integration Parameters dialog box.

In the TUI, enter the following text command in the console:

define/models/species/integration-parameters

When prompted with Enable Dynamic Mechanism Reduction?, answer with yes.

Note that it is not necessary to enable Chemistry Acceleration Expert mode in order to use Dynamic

Mechanism Reduction.

... Mechanism Reduction Parameters

... Monitoring and Postprocessing Dynamic Mechanism Reduction

... Using Dynamic Mechanism Reduction Effectively

In ANSYS Fluent, Dynamic Mechanism Reduction is controlled by the error tolerance and the target

species list, as described below.

Error Tolerance

(  in Equation . in the Fluent Theory Guide).The default value for error tolerance  is ., which should

work well for most simulations, balancing speed and accuracy. However, a larger tolerance may be sufficient

for some simulations (for example, steady-state simulations with moderate accuracy requirements), while

a smaller tolerance may be required in other cases with stricter accuracy requirements (for example,

modeling auto-ignition delay times for a highly complex fuel). In general, a larger tolerance yields faster,

but less accurate simulations.

The error tolerance can be adjusted through the GUI or TUI as follows:

In the GUI, set Error Tolerance to the desired value in the Mechanism Reduction Parameters group

box in the Integration Parameters dialog box.

In the TUI, enter the following text command: define/models/species/integration-para-

meters.When prompted with Mechanism Reduction Error Tolerance, enter the desired

tolerance (a positive, nonzero value) or press Enter to retain the default value.

Note

In the TUI, you can also enable Chemistry Acceleration Expert mode, other chemistry accel-

eration methods, and specify ODE integrator parameters (see Using ISAT (p. ) for details

about these parameters).

Chemistry Acceleration Expert mode should only be enabled if you want to modify the default

target species list.

Target Species List

As described in the Dynamic Mechanism Reduction in the Fluent Theory Guide, the target species are those

species that you want to predict most accurately.The default number of target species

is .The

first default target species is hydrogen radical. DRG will add two other species with the largest mass

fractions to complete the target species list at each flow time step or iteration. DRG will then identify all

other species that must also be included in the mechanism in order to accurately model these targets.

Although you should rarely need to alter the default target species list, ANSYS Fluent provides an

option to specify target species of your choice. The designated target species can be specified only

in the TUI when Chemistry Acceleration Expert mode is enabled. Enter the text command

define/models/species/integration-parameters and then answer yes when

prompted with Enable Chemistry Acceleration expert?.

ANSYS Fluent provides the ability to explicitly specify target species. From your mixture material list,

you can select any number

of target species to be included in the kinetics mechanism. In case

no targets were selected (

) or the number of user-selected targets

is less than the minimum

number of target species

(

), the DRG algorithm will add the (

) species

with the largest mass fractions to the target species list.

As discussed in the Dynamic Mechanism Reduction in the Fluent Theory Guide, there is an option to

) species

remove a species from the target list whenever its mass fraction is below a specified threshold. This

option is disabled by default in ANSYS Fluent (that is, the default value for minimum mass fraction is

).

When specifying Target Species List, you will receive the following prompts in the console:

.

Minimum number of target species []

Enter the desired number of targets.

.

Minimum mass fraction of target species []

Enter minimum allowable target mass fraction.

The current target species list will be displayed in the console window (for example, the console

output for the default target species consisting of hydrogen radical will be Current target

species list = (h)).

.

Enter target species list...

Species name [""]

Enter target species name, for example, "ch4".

Important

You must enter the complete name of the species as it appears in the Chemical Formula

field in the Create/Edit Materials dialog box within quotes (" ").

After you enter the first target species, you will be prompted to specify the second one, and so

on, until you press Enter to complete the setup.

Note, that if you have entered  for the minimum number of target species

and have not

provided any target species (that is, the number of user-selected targets,

, is zero), ANSYS

Fluent will automatically select the three species with the largest mass fraction and use them as

the target species in the DRG algorithm.

When Chemistry Acceleration expert is enabled in the TUI, two additional field variables are available

to be monitored or examined in postprocessing:

DRG Reduced Number of Species in the Species… category

DRG Reduced Number of Reactions in the Reactions... category

These field variables quantify the size of the reduced mechanism at each cell or particle in the domain

(the number of retained species and reactions, respectively).

When you use DMR in combination with ISAT, ANSYS Fluent will report values of zero for DRG Reduced

Number of Species and DRG Reduced Number of Reactions for those cells where the ANSYS solver

computed the solution using table lookup instead of direct integration in the ISAT algorithm. A cell

value of zero DRG Reduced Number of Species does not imply that the DMR algorithm eliminated

all species from the mechanism; rather, it indicates that the ANSYS solver performed ISAT table lookup

to obtain the chemistry solution at the cell.

If you want to view the cells for which ISAT table lookup was performed in the last iteration or time

step, display the DRG Reduced Number of Species plot clipped to a range of  to . (Make sure that

the Node Value option is deselected in the postprocessing dialog boxes.)

If you want to view the cells for which DMR was performed in the last iteration or time step, display

the DRG Reduced Number of Species plot clipped to a range of  to a global maximum value (as it

appears in the Max field when Global Range is selected in the postprocessing dialog boxes).

Note

The DMR postprocessing field variables are not stored in the data file and, hence, will not

Note

be available for postprocessing in the next session. If you want to postprocess these variables

in your next session, read the data file and perform a single iteration or time step (for steady-

state or transient simulations, respectively) in order for the DMR data to be calculated and

available for viewing.

As described in Dynamic Mechanism Reduction in the Fluent Theory Guide, mechanism reduction is

performed at each cell or particle, once per time step (for transient simulations) or per flow iteration

(for steady-state simulations). It is assumed that the reduced mechanism created for the starting con-

ditions will remain valid for the entire transport time step over which the chemistry ODE is integrated.

If the chemistry integration time interval is very large, the chemical state can change significantly,

degrading the accuracy of the reduced mechanism. In some cases (particularly transient simulations

such as ignition) it may be necessary to enforce smaller flow time steps in order to effectively use

Dynamic Mechanism Reduction. In this way the reduced mechanisms are updated more frequently to

match the changing chemical states.

Note that Dynamic Mechanism Reduction works best when there are significant regions in a computa-

tional domain and/or times during a simulation with relatively low chemical activity (for example, low

temperature, low mixing of fuel/oxidizer, low concentrations of reactive species, and so on). Consider

a simple opposed flow diffusion flame problem with pure fuel as one stream and pure oxygen as the

other stream. Large mechanisms (which, depending on the error tolerance, may be close to the full

mechanism size) will likely be used in the mixing region where the flame is located, while smaller

mechanisms would be used elsewhere in the domain. You should not expect much speed-up if a very

large fraction of your grid cells (for example, %) are in the flame region.

In steady-state simulations, you can improve the solution time by first running to convergence with

a larger error tolerance , and then restarting the simulation repeatedly, gradually decreasing the error

tolerance  until you reach the desired accuracy level. For example, if you first converge the solution

with the error tolerance

, then iterate the solution further to convergence with the lower error

tolerance,

, and then with the desired error tolerance

, you will generally be able to

achieve faster convergence than iterating from initial conditions with the error tolerance

.

Important

As described in Mesh Partitioning and Load Balancing (p. ), you can select portions of

the simulation to consider when performing dynamic load balancing in multiprocessor

simulations. When using the Dynamic Mechanism Reduction along with ISAT, it is recom-

mended that you select the ISAT option in the Weighting tab of the Partitioning and Load

Balancing Dialog Box (p. ) when solving stiff chemistry. If ISAT is selected, the time re-

quired for solving chemistry will be factored in when assigning the computational cells to

each available processor; thus, more resources can be allocated for the cells with the larger

mechanisms.

The Chemistry Agglomeration method reduces the number of calls to the computationally expensive

ODE integrator by clustering cells with similar compositions. The size of these clusters is determined

by the agglomeration parameters Error Tolerance (

) and Temperature Bin (

) in the Integration

Parameters dialog box. Larger values of

and

result in a larger number of agglomerated cells,

fewer calls to the reaction integrator, increased run-time speed, but greater error.

You can also set the chemistry agglomeration parameters using the text user interface (TUI) command

define/models/species/integration-parameters. Once you enable agglomeration chemistry,

ANSYS Fluent prompts you for Agglomerate Chemistry Error Tolerance and Agglomerate

Chemistry Temperature Bin. Enter the desired values or press Enter to retain the default values

of . for Agglomerate Chemistry Error Tolerance and  for Agglomerate Chemistry

Temperature Bin.

More information can be found in Chemistry Agglomeration in the Fluent Theory Guide.

Important

The solution accuracy can be improved by decreasing the tolerances. Generally, it should

not be necessary to reduce the tolerances below . and  K.

Detailed kinetic mechanisms typically contain a multitude of intermediate species that far exceed the

number of major fuel, oxidizer, and product species. Chemical mechanism Dimension Reduction reduces

the number of intermediate species transport equations (called representative species) that are solved,

and reconstructs the ‘unrepresented’ species using chemical equilibrium assumptions.

Important

Since ANSYS Fluent is limited to a maximum of  transported species, the main use of

Dimension Reduction is to enable simulation with chemical mechanisms containing more

than  species.

Follow these steps to use Dimension Reduction:

Import your CHEMKIN mechanism. Note that you can import CHEMKIN mechanisms that contain more than

species.

Click the Integration Parameters button in the Species Model dialog box, and enable Dimension Reduction.

Set the Number of Represented Species.This must be greater than  and less than the number of species

in the full mechanism.The Number of Represented Species must also be less than  minus the number

of unrepresented elements (the number of chemical elements in the unrepresented species). A larger

Number of Represented Species will increase accuracy, but also increase computational expense.The

default of  has been chosen to provide a good compromise between accuracy and speed.

Select the Full Mechanism Material Name, which is typically the name of the CHEMKIN mechanism that

you imported. ANSYS Fluent can store several imported CHEMKIN mechanisms in different mixture materials

whose mechanisms you are not using. However, since mechanisms are typically large, you should delete

unused mixtures to reduce memory requirements.

Set the boundary and initial fuel and oxidizer, as well as product species, as represented species.These are

set in the Fuel/Oxidizer Species list. Note that you can force other species to be represented by selecting

them here. Species of interest, especially species that are not near chemical equilibrium, such as pollutants,

and their associated intermediate species in the mechanism should also be included. Intermediate species

that occur in large mass fractions relative to the fuel and oxidizer species should be included, as well as

species important in the chemical pathway. For example, for methane combustion in air, CH3 should be in-

cluded as a represented species since CH4 pyrolizes to CH3 first.

Click Calculate Reduced Dimension Mixture.This will create a new mixture material called reduced-

dimension-mixture, which contains the represented species as well as proxy ’species’ for the unrepres-

ented elements.These unrepresented elements have “u" prepended to the element name.You should

never rename the reduced-dimension-mixture mixture material, or select another mixture as the active

material, while Dimension Reduction is enabled.

Continue with the setup, solution, and postprocessing as for other detailed chemistry cases. Note that the

boundary and initial mass fraction of unrepresented elements should always be zero.The entries for the

unrepresented element mass fractions are disabled in the ANSYS Fluent GUI.

For postprocessing, the unrepresented elements are available in the Species list as the element name

with “u" prepended. All species in the full mechanism, consisting of both represented and unrepresented

species, are available in the Full Mechanism Species... category of the postprocessing dialog boxes.

After you obtain a preliminary solution with Dimension Reduction, it is recommended that you check

the magnitude of all unrepresented species, which are available in the Full Mechanism Species... option

in the Contours dialog box. If the mass fraction of any unrepresented species is larger than other rep-

resented species, you should repeat the simulation with this species included in the represented species

list. In turn, the mass fraction of all unrepresented elements should decrease.

Note

Note that Dimension Reduction is only available with ISAT. Dimension Reduction is initially

comparable in speed to a simulation with the full mechanism, but iterations become signi-

ficantly faster at later times when the ISAT table is populated.

For information about the theory of this option, see Chemical Mechanism Dimension Reduction in the

The Dynamic Cell Clustering (DCC) method is available with the ANSYS CHEMKIN-CFD solver. DCC groups

computational cells with similar temperatures, pressures, and initial species mass fractions into clusters.

To use the DCC method, select Dynamic Cell Clustering in the Integration Parameters dialog box.

The following parameters are available for controlling dynamic cell clustering:

Max.Temperature Dispersion (default = K)

Max. Equiv. Ratio Dispersion (default =.)

Using Dynamic Cell Clustering

Max. Clusterization (default = ) and Min. Clusterization (default = )

These parameters limit the number of generated clusters and allocate the required amount of memory

in your analysis.

Reactants Threshold (mass fraction) (default = 1e-)

If the computed value of the species mass fraction is above the specified threshold, then the solver

calculates the clusterization parameters; otherwise, it is considered to be zero.

The default values for these parameters have been found to provide accurate results for a wide range

of combustion cases. Varying these parameters may affect the computational cost. For example, reducing

maximum temperature and equivalence ratio of dispersions increases the number of clusters, which

leads to a higher CPU cost.

For background information about DCC, refer to Dynamic Cell Clustering with ANSYS Fluent CHEMKIN-

CFD Solver in the Fluent Theory Guide.

.. Using Dynamic Adaptive Chemistry with ANSYS Fluent CHEMKIN-

CFD Solver

Note

Dynamic Adaptive Chemistry is not compatible with ISAT.

The Dynamic Adaptive Chemistry method is controlled by the following parameters:

DAC Error Tolerance: Controls the level of accuracy.

A larger tolerance would tend to lower the accuracy but might speed up the computation. The

default value for DAC error tolerance is ., which should be suitable for most cases.

DAC target species: Are the initial species to be tracked by the DAC algorithm.

You can select the target species for your analysis in the Select DAC Target Species dialog box

that opens when you click Select Target Species in the Integration Parameters dialog box.

Figure . : The Select DAC Target Species Dialog Box

For both diesel and gasoline surrogate fuels, CO, HO2, and fuel species are an effective choice

for the target species ( and ). By default, only co and ho2 are selected as the DAC target

species. You must also select fuel species for your analysis.

To modify the DAC target species list:

– To remove the species from the Selected Species multiple-selection list, select it and click Remove.

– To add the species back to the Selected Species list, select it in the Unselected Species multiple-

selection list and click Add.The species will be moved from the Unselected Species list to the Selec-

ted Species list.

For information about the theory of this method, see Dynamic Adaptive Chemistry with ANSYS Fluent

CHEMKIN-CFD Solver in the Fluent Theory Guide.

Using Dynamic Adaptive Chemistry with ANSYS Fluent CHEMKIN-CFD Solver

Chapter : Modeling Engine Ignition

This chapter discusses how to use the engine ignition models available in ANSYS Fluent in the following

sections. For information about the theory behind these ignition models, see Engine Ignition in the

.. Spark Model

.. Autoignition Models

.. Crevice Model

The spark model in ANSYS Fluent will be described in the context of the premixed and partially premixed

combustion models, including the species transport model. For information regarding the theory of

this model, see Spark Model in the Theory Guide. Information regarding the use of this model is detailed

... Using the Spark Model

... Using the ECFM Spark Model

You can model a single spark or multiple sparks. To use the spark model, perform the following steps:

. Select Transient from the Time list in the General task page (or from the General → Analysis Type in

the tree).

. In the Species Model dialog box, select one of the following reaction models:

Edit...

Under Model, select Species Transport, and under Reactions, enable Volumetric.

Under Model, select Premixed Model with the C Equation or G Equation model enabled. See Setting

Up the C-Equation and G-Equation Models (p. ) for more information.

The Spark Ignition model will now appear in the Models task page and under the Models tree

item.

Important

When you read in a R14. case file, ANSYS Fluent will revert to the R14. spark model

by default. To switch to the current spark model, you can either

open the Spark Ignition dialog box, or

use the TUI define/models/species/spark-model command.

You can also use the TUI define/models/species/spark-model command to

revert back to the R14. spark model.

. Define sparks for your case using the Spark Ignition dialog box (see Figure . :The Spark Ignition Dialog

Box (p. )).

Setup → Models → Species → Spark Ignition

Edit...

Figure . : The Spark Ignition Dialog Box

. Specify the Number of Sparks you would like to include in your simulation.You can define up to

sparks.

. While you can define several sparks, you can choose which ones to turn on using the On option.

. Enter the Name of the spark, or simply keep the default name.

sparks.

. Click the Define... button to open the Set Spark Ignition dialog box (Figure . :The Set Spark Ignition

Dialog Box (p. )), where you will set the parameters of the selected spark ignition models.

Modeling Engine Ignition

Figure . : The Set Spark Ignition Dialog Box

. Set the spark model parameters.

Set X,Y, and Z coordinates of the spark center and the Initial Radius of the spark kernel in the Spark

Location group box.

Enter Start Time and Duration in the Spark Parameters group box.

Important

When the in-cylinder model is turned on, the Start Time is entered in crank angle

degrees instead of seconds, while the spark Duration is still in seconds. The value

you enter for Start Time is for one complete engine cycle. In subsequent cycles, the

spark is enabled according to Equation . (p. ), where

corresponds to the

spark start crank angle.

(optional) Set Energy to a positive value if you want to model the higher temperature levels within the

spark kernel.The energy input will be evenly distributed across the specified spark duration.This energy

is not required to initiate combustion.The spark model will control the spark kernel growth and com-

bustion progress. For this reason the default energy input is zero. If you specify extra energy here, it

will raise the kernel temperature beyond that given by the combustion process.

Select the Flame Speed Model from the drop-down list. For details of these models see Spark Model

Theory in the Fluent Theory Guide.

Spark Model

When the Extended Coherent Flamelet Model (see Setting Up the Extended Coherent Flame Mod-

el (p. )) is selected in the Species Model dialog box, the Set Spark Ignition dialog box will exhibit

additional ECFM Spark Model options, as shown in Figure . : The Set Spark Ignition Dialog Box

Displaying the ECFM Spark Model Options (p. ).

Figure . : The Set Spark Ignition Dialog Box Displaying the ECFM Spark Model Options

In addition to specifying the variables mentioned in Using the Spark Model (p. ), you can select

from one of the following ECFM Spark models:

Turbulent

Zimont (default)

Constant Value

User Defined Sigma Source

This controls the way in which the value of the flame surface density is calculated. More details are

given in ECFM Spark Model Variants in the Fluent Theory Guide.

If you choose Constant Value you will be required to specify the value for flame surface density. If

you choose User Defined Sigma Source you will need to choose the hooked user-defined function

to apply a custom source term to the ECFM equation within the volume of the spark ignition kernel.

For more detail about this user-defined function, refer to Hooking DEFINE_ECFM_SPARK_SOURCE

UDFs in the Fluent Customization Manual.

Autoignition phenomena in engines are due to the effects of chemical kinetics of the reacting flow inside

the cylinder. There are two types of autoignition models considered in ANSYS Fluent:

knock model in spark-ignited (SI) engines

ignition delay model in diesel engines

For information regarding the theory behind autoignition models, see Autoignition Models in the Theory

Guide. Using the Autoignition Models (p. ) describes how to use the autoignition models in ANSYS

Fluent.

... Using the Autoignition Models

To use the autoignition model, perform the following steps:

the tree).

. Select an appropriate reaction model in the Species Model dialog box.

Edit...

. The models in the Species Model dialog box that are compatible with the autoignition model are Species

Transport, Premixed Combustion, and Partially Premixed Combustion.

The Autoignition model will now appear in the Models task page and under the Models tree

item.

Important

If you select Species Transport, you must also enable the Volumetric option in the Reactions

group box.

The Premixed Combustion and Partially Premixed Combustion models are only available

for turbulent flows using the pressure-based solver.

. Select the Autoignition model.

Setup → Models → Species → Autoignition

Edit...

If Species Transport is selected in the Species Model dialog box, you can only select the Ignition

Delay Model.

Autoignition Models

Figure . : The Ignition Delay Model in the Autoignition Model Dialog Box

If Premixed Combustion is selected in the Species Model dialog box, you can only select the Knock

Model.

Figure . : The Knock Model in the Autoignition Model Dialog Box

If Partially Premixed Combustion is selected in the Species Model dialog box, you can select either

Model.

the Knock Model or the Ignition Delay Model.

. When the Ignition Delay Model is enabled, the dialog box expands to include the modeling parameters

for this model (Figure . :The Ignition Delay Model for the Partially Premixed Combustion Model (p. )).

The two correlation options that exist with this model are Hardenburg and Generalized. Depending on

which correlation option is selected, the appropriate modeling parameters will appear in the dialog box.

Figure . : The Ignition Delay Model for the Partially Premixed Combustion Model

The Hardenburg option is typically used for heavy duty diesel engines.With this option, the following

parameters are available:

– Pre-Exponential

– Pressure Exponent

– Activation Energy

– Cetane Number

For the Species Transport model, Fuel Species is selected from the drop-down list.

The Generalized option is described by Equation . in the Theory Guide.With this option, the fol-

lowing parameters are available:

– Temperature Exponent

– RPM Exponent

– Equivalence Ratio Exponent

– Octane Number

– Octane Number Exponent

Default values of these parameters can be found in Default Values of the Variables in the Hardenburg

Correlation in the Fluent Theory Guide.

. When the Knock Model is enabled, the dialog box expands to include modeling parameters for this

model (Figure . :The Knock Model with the Partially Premixed Combustion Model Enabled (p. )).The

two correlation options that exist with this model are Douaud and Generalized. Depending on which

correlation option is selected, the appropriate modeling parameters will appear in the dialog box.

Figure . : The Knock Model with the Partially Premixed Combustion Model Enabled

The Douaud option is used for knock in SI engines.The modeling parameters that are specified in the

Autoignition Model dialog box for this option are the Pre-Exponential, Pressure Exponent, Activation

Temperature, Octane Number, and Octane Exponent (Equation . in the Theory Guide).

The Generalized option (Equation . in the Theory Guide) in the knock model requires the same

parameters as in the ignition delay model.

For information regarding the theory behind the crevice model, see Crevice Model in the Theory Guide.

Using the crevice models in ANSYS Fluent are described in the following sections:

... Using the Crevice Model

... Crevice Model Solution Details

... Postprocessing for the Crevice Model

An optical experimental engine  [] (p. ) is used below to show a working example of how to use

the crevice model as it is implemented in ANSYS Fluent. The mesh at ten crank angle degrees before

top center is shown in Figure . : Experimental Engine Mesh (p. ).

Figure . : Experimental Engine Mesh

The following example shows the necessary steps to enable the crevice model for a typical in-cylinder

flow.

. From the > prompt, enter the define/models menu by using the following text command:

define → models

flow.

. Enable the crevice model, as follows:

/define/models   crevice-model?

Enable crevice model? [no] yes

/define/models

acoustics/                multiphase/                   species/

addon-module              noniterative-time-advance? steady?

axisymmetric? nox? unsteady-1st-order?

crevice-model-controls/   radiation/                    unsteady-2nd-order?

crevice-model? solidification-melting? viscous/

dpm/                      solver/

energy? soot?

frozen-flux? sox?

. Enter the ring pack geometry:

/define/models   crevice-model-controls

Cylinder bore (m) [.] .

Piston to bore clearance (m) [.0e-] .08e-

Piston crevice temperature (K) []

Piston sector angle (deg) []

Crevice Model

Ring discharge coefficient [.] .

Pressure in crankcase (exit pressure) (Pa) []

Write  out  crevice  data  to  a  file? [no]   yes

output file name ["crev.out"]

Available  wall  threads  are:  (wall. wall  wall-)

Leaking  wall []   wall.

Shared boundary [] wall-

Selected  boundary  threads  :  (wall. wall-)

Use  these  zones? [yes]   yes

Solve crevice model ? [no] yes

Number of rings []

Width  of  ring  number    is:  [.]

Thickness  of  ring  number    is:  [.]

Spacing  of  ring  number    is:  [.]

Land  Length  for  ring  number    is:  [.]

Top  Gap  of  ring  number    is:  [6e-]

Middle  Gap  of  ring  number    is:  [4e-]

Bottom  Gap  of  ring  number    is:  [6e-]

Initial  conditions  in  ring  pack

Pressure    is:  [.]

Pressure    is:  []

A fast way to set up multiple rings in the ring pack is to specify only one ring and enter the geo-

metry. Once the ring geometry is entered, invoke the crevice-model- controls menu a

second time and specify the number of rings desired. When the number of rings changes, the

geometry from the first ring is copied to all subsequent rings. Default values can be taken for the

rest of the way through the menu structure.

A summary of the crevice model is printed out by entering the (crevice-summary) command

at the command prompt:

>(crevice-summary)

crevice/n-rings  :

crevice/ring-width  :  (. . .)

crevice/ring-thickness  :  (. . .)

crevice/ring-mass  :  (. . .)

crevice/ring-spacing  :  (. . .)

crevice/land-length  :  (. . .)

crevice/top-ring-gap  :  (6e-  6e-  6e-)

crevice/mid-ring-gap  :  (4e-  4e-  4e-)

crevice/bot-ring-gap  :  (6e-  6e-  6e-)

crevice/piston-temperature  :

crevice/sector-angle  :

crevice/mid-gap-cd  :  .

crevice/exit-pressure  :

crevice/threads  :  (  )

names  of  crevice/threads  :  (wall. wall-)

crevice/unit-roundoff  :  .9604645e-

crevice/piston-bore-clearance  :  .08e-

crevice/write? :  #t

crevice/output-file  :  crev.out

crevice/solve? :  #t

crevice/enabled? :  #t

crevice/pressures  :  (. . .    )

The under-relaxation factor for the crevice model source terms can be found in the Solution Controls

task page. The default value for Crevice Model Sources is ., which has been found to work well for

motored engine simulations. Once the crevice model is enabled, the solution proceeds normally.

Solution →

Controls

Solution →

Solution →

A plot of cylinder mass with and without the crevice model during the motored engine simulation is

shown in Figure . : Cylinder Mass vs. Crank Angle (p. ). The rate of mass loss from the crevice is

proportional to the pressure difference between the cylinder and the crankcase pressure defined in

the text interface.

Figure . : Cylinder Mass vs. Crank Angle

A plot of cylinder pressure with and without the crevice model for the same engine simulation is shown

in Figure . : Cylinder Pressure vs. Crank Angle (p. ). The effect of the mass loss from the crevice

is to lower the peak pressure in proportion to the total mass loss from the cylinder.

Figure . : Cylinder Pressure vs. Crank Angle

.... Using the Crevice Output File

The pressure in the top ring land is defined as the cylinder pressure (that is, the pressure in the cells

defining the ring landing). Intermediate pressures are available at any point during the ANSYS Flu-

ent session through the (crevice-summary) command as previously shown. If the optional data

file output is chosen in the crevice-model-controls, the intermediate pressures in the defined

crevices are printed to the file crev.out at the start of each new time step. The format of the file

# crank (deg) data-press[..................] total_mdot

.95500e+ .16650e+ .01325e+ .01325e+ .01325e+ .01325e+ .01325e+ .01325e+ .

.96000e+ .09945e+ .06794e+ .81553e+ .04111e+ .48582e+ .02202e+ .01325e+ -.

.96500e+ .17787e+ .13070e+ .88242e+ .07960e+ .53544e+ .03526e+ .01325e+ -.

.97000e+ .17434e+ .19065e+ .88060e+ .11705e+ .53475e+ .04830e+ .01325e+ -.

.97500e+ .17652e+ .24777e+ .88299e+ .15286e+ .53668e+ .06081e+ .01325e+ -.

.98000e+ .17937e+ .30215e+ .88594e+ .18711e+ .53900e+ .07283e+ .01325e+ -.

where the first column is the current flow time (or crank angle), and the next

columns are the

ring pressures (where

is the number of crevice volumes, or

), including the face pressure

on the crevice cell, and the defined pressure at the crevice exit. The final column is the mass flow

past the top ring. This file is currently formatted so that it can be read into the free Gnuplot plotting

package, which is available at www.gnuplot.info.

To read the crevice output file into ANSYS Fluent as a data file, you will need to put each column of

the crevice output file in its own individual file. The first three lines of each column of the data file

should be of the following form:

"Title"

"X-Label" "Y-Label"

where the title,

label, and -label strings are enclosed by double quotes and the third line of the

file contains four zeros. The lines following the first three lines of the file are the columns you want

to plot. For example, to plot column  versus column  of the crevice model output file in ANSYS

Fluent, you would enter the following commands in a Linux terminal:

cat > crev_col_1_3.dat

"Column  vs Column "

"Crank Angle (deg)" "Pressure behind ring  (Pa)"

ctrl-d

where ctrl-d is the end-of-file character made holding down the Ctrl key and pressing d (Ctrl+d).

To append columns  and  to this file, enter the following:

tail + crev.out | awk ’{print $, $}’ >> crev_col_1_3.dat

The file crev_col_1_3.dat can now be read into ANSYS Fluent using the File XY Plot Dialog

Box (p. ). See XY Plots of File Data (p. ) for details about creating -  plots. For Windows users,

the file crev.out can be imported into Excel for plotting purposes without any modification.

A Gnuplot plot of the pressure in the ring pack crevices for the above engine simulation is shown

in Figure . : Crevice Pressures (p. ). After an initial transient period where the flows in the network

settle down, Figure . : Crevice Pressures (p. ) shows that the pressure in the ring crevices follows

the cylinder pressure in form, though with pressure magnitudes that are controlled by the ring pack

geometry.

Figure . : Crevice Pressures

Chapter : Modeling Pollutant Formation

This chapter discusses how to use the models available in ANSYS Fluent for modeling pollutant formation.

For information about the theory behind the models in ANSYS Fluent, see Pollutant Formation in the

Information is presented in the following sections:

.. NOx Formation

.. SOx Formation

.. Soot Formation

.. Using the Decoupled Detailed Chemistry Model

The following sections describe how to use the NOx models in ANSYS Fluent. For information about

the theory behind the NOx models in ANSYS Fluent, see NOx Formation in the Theory Guide.

... Using the NOx Model

... Solution Strategies

... Postprocessing

.... Decoupled Analysis: Overview

NOx concentrations generated in combustion systems are generally low. As a result, NOx chemistry

has negligible influence on the predicted flow field, temperature, and major combustion product

concentrations. It follows that the most efficient way to use the NOx model is as a postprocessor to

the main combustion calculation.

The recommended procedure is as follows:

. Calculate your combustion problem using ANSYS Fluent as usual.

Important

The premixed combustion model is not compatible with the NOx model.

Important

If you plan to use the ANSYS Fluent selective non-catalytic reduction (SNCR) model for

NOx reduction, you must first include ammonia NH3 or urea CO(NH2) (depending upon

which reagent is employed) as a fluid species in the main combustion calculation and

define appropriate species injections, as described later in this section. See Defining

the Species in the Mixture (p. ) for details about adding species to your model and

Setting Initial Conditions for the Discrete Phase (p. ) for details about creating injec-

tions.

. Enable the desired NOx models (thermal, prompt, fuel, and/or N2O intermediate NOx, with or without

reburn), define the fuel streams (for prompt NOx and fuel NOx only), and set the appropriate parameters,

as described in this section.

Setup → Models → Species → NOx

Edit...

. Define the boundary conditions for NO (and HCN, NH3, or N2O if necessary) at flow inlets.

Setup →

. (steady state only) In the Equations Dialog Box (p. ), turn off the solution of all variables except species

NO (and HCN, NH3, or N2O, based on the model selected).

Solution →

. (transient cases only) In the Run Calculation task page, select Postprocess Pollutants and adjust Max

Post Iterations/Time Step as needed.

Solution →

. Perform calculations until convergence (that is, until the NO—and HCN, NH3, or N2O, if solved—species

residuals are below -).

Solution →

. Review the mass fractions of NO (and HCN, NH3, or N2O) by generating graphical plots or alphanumeric

reports in the usual way.

. Save a new set of case and data files, if desired.

Inputs specific to the calculation of NOx formation are explained in the remainder of this section.

.... Enabling the NOx Models

To enable the NOx models and set related parameters, you will use the NOx Model Dialog Box (p. )

(for example, Figure . : The NOx Model Dialog Box (p. )).

Edit...

Modeling Pollutant Formation

Edit...

Figure . : The NOx Model Dialog Box

In the Formation tab, select the NOx models under Pathways to be used in the calculation of the

NO and HCN, NH3, or N2O concentrations:

To enable thermal NOx, turn on the Thermal NOx option.

To enable prompt NOx, turn on the Prompt NOx option.

To enable fuel NOx, turn on the Fuel NOx option.

Important

When using the non-premixed combustion model, the following limitation exists for the

Fuel NOx option:

– The Fuel NOx option is only available if the DPM model is also enabled.

To enable the formation of NOx through N2O intermediate, turn on the N2O Intermediate option. (Note

that the N2O option will not appear until you have enabled one of the other NO models listed above.)

Your selection(s) under Pathways will enable the calculation of thermal, prompt, fuel, and/or N2O-

intermediate NOx in accordance with the chemical kinetic models described in Thermal NOx Formation

through NOx Formation from Intermediate N2O in the Theory Guide. Mean NO formation rates will

be computed directly from mean concentrations and temperature in the flow field.

NOx Formation

.... Defining the Fuel Streams

When modeling fuel NOx formation, ANSYS Fluent allows you to define up to three separate fuel

streams, and to select

fuel sources for each fuel stream.

You can define multiple fuel streams to include in your model with the following configurations:

Solid and liquid fuels (combusting particle and droplet) both contributing to fuel NOx.

Two or three solid fuels with different -content and NOx model parameters (two or three combusting

particles), for example coal blends, coal-biomass cofiring, and so on.

Two or three liquid fuels with different -content and NOx model parameters (two or three droplet

or multicomponent particles).

Gas and solid (or droplet) fuel both contributing to fuel NOx.

In addition, you can model one solid fuel contributing to NOx in the presence of another re-

acting solid particle not containing any

(for example, sorbent injection in a coal furnace or

calcination reaction in cement kiln) by specifying the active

fuel source for NOx formation.

For this configuration, you will not need to define multiple fuel streams in your model.

If Fuel NOx is enabled in the Pathways group box in the Formation tab, perform the following steps

to define multiple fuel streams:

. Specify the Number of Fuel Streams in the Fuel Streams group box.

Note

You are allowed up to three separate fuel streams.

. Define the first fuel stream.

a.

Select the fuel stream to be defined by using the arrow keys of the Fuel Stream ID field.

b. Select the Fuel Type in the Fuel tab for the Formation Model Parameters.

c.

If your Fuel Type is Liquid or Solid, select the N sources from the Fuel Sources list.

If the Fuel Type is Solid and you have defined multiple injections with different combusting particle

materials in your reacting flow calculation, the available combusting particle materials will be listed

in the Fuel Sources list. Select one or more materials from the list to be included as fuel sources

in the Fuel NOx calculation.Your selection will be used to determine the char burnout rate

and

volatile release rate

in the coal fuel NOx formation rate models described in Fuel NOx from

and

Coal in the Theory Guide. Make sure to deselect all combusting particle materials that do not

contribute to NOx.

If the Fuel Type is Liquid and you have defined multiple injections with different droplet or mul-

ticomponent particle materials in your reacting flow calculation, the available materials will be

listed in the Fuel Sources list. Select one or more materials from the list to be included as fuel

sources in the Fuel NOx calculation.Your selection will be used to determine the fuel release rate

in the liquid fuel NOx formation rate models described in Fuel NOx from Intermediate Hydrogen

Cyanide (HCN) and Fuel NOx from Intermediate Ammonia (NH3) in the Theory Guide. Make sure

to deselect all droplet and multicomponent materials that do not contribute to NOx.

d. If you are also modeling Prompt NOx, select the fuel species from the Fuel Species list.You cannot

select more than  fuel species for each fuel stream, and the total number of fuel species selected

for all the fuel streams combined cannot exceed .You can define the same, or different Fuel Species,

Fuel Carbon Number and Equivalence Ratio for each stream.The Fuel Carbon Number and

Equivalence Ratio can be modified in the Prompt tab under Formation Model Parameters.

e. If the Fuel Type in your model is Gas, select one or more materials from the Fuel Species list.Your

selection will be used to determine the mean limiting reaction rate

in the gaseous fuel NOx

formation rate models described in Fuel NOx from Intermediate Hydrogen Cyanide (HCN) and Fuel

NOx from Intermediate Ammonia (NH3) in the Theory Guide. If you are also modeling Prompt NOx

formation, the same fuel selection will apply also for the prompt NOx model.

f.

Set the other parameters associated with your selected pathway(s) in the Prompt and/or Fuel tabs

under Formation Model Parameters. See Setting Prompt NOx Parameters (p. ) and Setting Fuel

NOx Parameters (p. ) for details.

. Repeat steps . (a)–. (f) for each additional fuel stream.

Important

The gaseous fuel option is available only when the species model is enabled.

Important considerations should be made when reading case and data files set up in a version

of ANSYS Fluent . or earlier:

– When reading a case and data file with multiple injection materials that was set up in ANSYS

Fluent version . or earlier, ANSYS Fluent will initialize the injection material specific fuel

N sources for the fuel NOx model. ANSYS Fluent will perform a DPM iteration when the flow

iterations are initiated.

– When reading a case file that was set up in a version older than ANSYS Fluent . with

multiple fuel streams defined for the Fuel NOx model, you must review the setup and select

the N sources from the Fuel Sources list.

Figure . : The NOx Model Dialog Box Displaying the Fuel Streams

.... Specifying a User-Defined Function for the NOx Rate

You can choose to specify a user-defined function for the rate of NOx production. By default, the rate

returned from the UDF is added to the rate returned from the standard NOx production options, if

any are selected. You also have the option of replacing any or all of ANSYS Fluent’s NOx rate calculations

with your own user-defined NOx rate.

In addition to or instead of using the UDF to specify the NOx rate, you can use it to specify custom

values for the maximum limit (

) that is used for the integration of the temperature PDF (when

temperature is accounted for in the turbulence interaction modeling).

To use a UDF to add a rate to ANSYS Fluent’s NOx rate calculations, you must compile and load the

desired function, and then select it from the NOx Rate drop-down list in the User-Defined Functions

group box in the Formation tab. After you have selected the UDF, you have the following options:

You can specify that your custom rate is added to the ANSYS Fluent NOx rate calculations, by retaining

the default selection of Add to Fluent Rate in the UDF Rate group box for the appropriate NOx formation

pathway(s) (for example, in the Fuel tab).

You can replace the ANSYS Fluent NOx rate calculations with your custom rate, by selecting Replace

Fluent Rate in the UDF Rate group box for the appropriate NOx formation pathway(s) (for example, in

the Fuel tab).

You can specify custom values for

, by selecting user-defined from the Tmax Option drop-down

list in the Turbulence Interaction Mode tab.

See the Fluent Customization Manual for details about user-defined functions.

.... Setting Thermal NOx Parameters

The

routines employ three methods for calculation of thermal NOx (as described in Method :

Equilibrium Approach in the Theory Guide). You will specify the method to be used in the Thermal

The

tab, under Formation Model Parameters in the NOx Model Dialog Box (p. ):

To choose the equilibrium method, select equilibrium in the [O] Model drop-down list.

To choose the partial equilibrium method, select partial-equilibrium in the [O] Model or [OH] Model

To use the predicted O and/or OH concentration, select instantaneous in the [O] Model or [OH] Model

Important

Note that the urea model uses the [OH] model.

If you hooked a user-defined function in the Formation tab, you can make a selection in the UDF

Rate group box to specify the treatment of the user-defined NOx rate:

Select Replace Fluent Rate to replace ANSYS Fluent’s thermal NOx rate calculations with the custom NOx

rate produced by your UDF.

Select Add to Fluent Rate to add the custom NOx rate produced by your UDF to ANSYS Fluent’s thermal

NOx rate calculations.

.... Setting Prompt NOx Parameters

Prompt NOx formation is predicted using Equation . and Equation . in the Theory Guide. For

each fuel stream specified in the Fuel Stream ID field in the Formation tab, set the parameters in

the Prompt tab under Formation Model Parameters in the NOx Model Dialog Box (p. ) in the

following manner:

Set the Fuel Carbon Number to specify the number of carbon atoms per fuel molecule.

Set the Equivalence Ratio as follows:

(.)

(.)

Select Replace Fluent Rate to replace ANSYS Fluent’s prompt NOx rate calculations with the custom NOx

Select Add to Fluent Rate to add the custom NOx rate produced by your UDF to ANSYS Fluent’s prompt

.... Setting Fuel NOx Parameters

When using the fuel NOx model, you must set the parameters in the Fuel tab under Formation

Model Parameters for each fuel stream specified in the Fuel Stream ID field in the Formation tab.

Select Replace Fluent Rate to replace ANSYS Fluent’s fuel NOx rate calculations with the custom NOx rate

produced by your UDF.

Select Add to Fluent Rate to add the custom NOx rate produced by your UDF to ANSYS Fluent’s fuel NOx

rate calculations.

If there is no NOx rate UDF or if you selected Add to Fluent Rate, you must define fuel parameters.

To begin, specify the fuel type in the following manner:

For solid fuel NOx, select Solid under Fuel Type.

For liquid fuel NOx, select Liquid under Fuel Type.

For gaseous fuel NOx, select Gas under Fuel Type.

Note that you can use only one of the fuel types for a given fuel stream. The Gas option is available

only when the Species Transport model is enabled (see Enabling Species Transport and Reactions

and Choosing the Mixture Material (p. )).

..... Setting Gaseous and Liquid Fuel NOx Parameters

If you have selected Gas or Liquid as the Fuel Type, you must also specify the following:

Select the intermediate species (hcn, nh3, or hcn/nh3/no) in the N Intermediate drop-down list.

Set the correct mass fraction of nitrogen in the fuel (kg nitrogen per kg fuel) in the Fuel N Mass Fraction

field.

Specify the overall fraction of the fuel N, by mass, that will be converted to the intermediate species

and/or product NO in the Conversion Fraction field.The Conversion Fraction for the N Intermediate

has a default value of .Therefore, any remaining N will not contribute to NOx formation.This is based

on the assumption that the remaining volatile N will convert to gas phase nitrogen. However, this has

very little effect on the overall mass fraction of gas phase nitrogen.Therefore, you do not have to solve

for nitrogen species when solving pollutant transport equations.

If you selected hcn/nh3/no as the intermediate, specify the fraction of the converted fuel N, by mass,

that will become hcn and nh3 under Partition Fractions.The fraction of fuel N that will become NO will

be calculated by the remainder.

Note that setting a partition fraction of  for both HCN and NH3 is equivalent to assuming that

all fuel N is converted to the final product NO, whereas a partition fraction of  for HCN and  for

NH3 is the same as selecting nh3 as the intermediate.

ANSYS Fluent will use Equation . and Equation . in the Theory Guide (for HCN) or Equa-

tion . and Equation . in the Theory Guide (for NH3) to predict NO formation for a gaseous

or liquid fuel.

Important

Important

Note that there is a limitation that must be considered when defining more than one liquid

fuel stream. See Defining the Fuel Streams (p. ) for details.

..... Setting Solid (Coal) Fuel NOx Parameters

For solid (coal) fuel, ANSYS Fluent will use Equation . and Equation . in the Theory Guide

(for HCN) or Equation . and Equation . in the Theory Guide (for NH3) to predict NO formation.

Several inputs are required for the coal fuel NOx model as follows:

Specify the mass fraction of nitrogen in the volatiles in the Volatile N Mass Fraction field.

Specify the overall fraction of the volatile , by mass, that will be converted to the intermediate species

and/or product NO in the Conversion Fraction field.

If you selected hcn/nh3/no as the volatile N intermediate, specify the fraction of the converted volatile

N, by mass, that will become hcn and nh3 under Partition Fractions.The fraction of volatile N that will

become NO will be calculated by the remainder.

Select the char N conversion path from the Char N Conversion drop-down list as no, hcn, nh3, or

hcn/nh3/no. Note that hcn or nh3 can be selected only if the same species has been selected as the in-

termediate species in the N Intermediate drop-down list.

Specify the mass fraction of nitrogen in the char in the Char N Mass Fraction field.

Specify the overall fraction of the char N, by mass, that will be converted to the intermediate species

If you selected hcn/nh3/no as the char N conversion, specify the fraction of the converted char N, by

mass, that will become hcn and nh3 under Partition Fractions.The fraction of char N that will become

NO will be calculated by the remainder.

Define the BET internal pore surface area (see BET Surface Area in the Theory Guide for details) of the

particles in the BET Surface Area field.

Important

Note that there are limitations that must be considered when defining more than one

solid fuel stream. See Defining the Fuel Streams (p. ) for details.

The following equations are used to determine the mass fraction of nitrogen in the volatiles and

char:

(.)

where

= release rate of fuel nitrogen in kg/s

= release rate of volatiles ( ) or char ( ) in kg/s

= mass fraction of nitrogen in volatiles or char

Let

= total nitrogen mass fraction in daf coal (that is, from daf ultimate analysis)

= char nitrogen as a fraction of total nitrogen

= mass fraction of volatiles in daf coal

= mass fraction of char in daf coal

Then the following should hold:

(.)

(.)

(.)

(.)

(.)

.... Setting N2O Pathway Parameters

The formation of NO through an N2O intermediate can be predicted by any of quasi-steady and

transported-simple methods, which can be specified in the N2O Path tab.

To choose the quasi-steady-state method, select quasi-steady in the N2O Model drop-down list.

Important

The transport equation for the species N2O will not be solved for N2O. However, N2O

will be updated at every iteration. Therefore, the residual values that appear for N2O are

always zero. Do not be alarmed if the solver keeps printing zero at each iteration.

To choose the simplified form of the N2O-intermediate mechanism, select transported-simple in the

N2O Model drop-down list. Here, the species N2O is added to the list of pollutant species, and its mass

fraction is solved via a transport equation.

The atomic O concentration will be calculated according to the thermal NOx [O] Model that you have

specified previously. If you have not selected the Thermal NOx pathway, then you will be given the

option to specify an [O] Model for the N2O pathway calculation. The same three options for the

thermal NOx [O] Model will be the available options.

Select Replace Fluent Rate to replace the NOx rate calculated by ANSYS Fluent using N2O intermediates

with the custom NOx rate produced by your UDF.

Select Add to Fluent Rate to add the custom NOx rate produced by your UDF to the NOx rate calculated

by ANSYS Fluent using N2O intermediates.

.... Setting Parameters for NOx Reburn

To enable NOx reduction by reburning, click the Reduction tab in the NOx Model Dialog Box (p. )

and enable the Reburn option under Methods. In the expanded portion of the dialog box, as shown

in Figure . : The NOx Dialog Box Displaying the Reburn Reduction Method (p. ), click the Reburn

tab under Reduction Method Parameters, where you can choose from the following options:

To choose the instantaneous method, select instantaneous [CH] in the Reburn Model drop-down list.

Important

Important

When you use this method, you must be sure to include the species CH, CH2, and CH3

in your problem definition. See NOx Reduction by Reburning in the Theory Guide for

details.

To choose the partial equilibrium method, select partial-equilibrium in the Reburn Model drop-down

list.You then must select the Reburn Fuel Species from the list of available species. ANSYS Fluent will

allow you select up to six reburn fuel species. Specify the Equivalent Fuel Type (ch4, ch3, ch2, or ch).

For example, if you choose methane as the reburn fuel, then the Equivalent Fuel Type would be ch4. If

you choose a reburn fuel such as hv_vol (a volatile component of coal), then you must specify the most

appropriate equivalent hydrocarbon fuel type so that the partial equilibrium model will be set up correctly.

Due to coal volatiles behaving very differently, it is important to select the correct equivalent fuel type.

You must first consider the volatile fuel composition, then check the C/H ratio to find the fuel that most

closely matches CH, CH2, CH3, or CH4 [] (p. ).While the method for best determining the equivalent

fuel is debatable, considering the C/H ratio of the fuel itself is a reasonable indicator.

Figure . : The NOx Dialog Box Displaying the Reburn Reduction Method

.... Setting SNCR Parameters

Prior to enabling reduction by SNCR, make sure that you have included in the species list nh3 (for

reduction by ammonia injection) and co<nh2> (for reduction by urea injection). See NOx Reduction

by SNCR in the Theory Guide for detailed information about SNCR theory.

. To enable NOx reduction by SNCR, click the Reduction tab in the NOx Model Dialog Box (p. ) and enable

the SNCR option under Methods, as shown in Figure . :The NOx Dialog Box Displaying the SNCR

Reduction Method (p. ).

Figure . : The NOx Dialog Box Displaying the SNCR Reduction Method

. In the SNCR tab under Reduction Method Parameters,set from the following options:

To have ammonia or urea included as a gas-phase pollutant species from the injection locations, select

gaseous in the Injection Method drop-down list.

If you plan to select this option for NOx postprocessing, then you must also include ammonia

or urea as a gas-phase species. Additionally, you must specify the mass fraction of ammonia or

urea at the respective inlet for the SNCR injection. You must include this set of inputs prior to

the main ANSYS Fluent combustion calculation.

To have ammonia included as a liquid-phase pollutant species from the injection locations, select liquid

in the Injection Method drop-down list. If urea is injected as a liquid solution, then select liquid in

the Injection Method drop-down list. Note that you must enable the DPM model with urea or ammonia

included as a material.

Note

All particle types such as droplets, combusting, and multicomponent particles are

compatible with the SNCR model.

If you plan to select this option for NOx postprocessing, then you must include NH3 as both a

gas-phase and liquid-phase species. Additionally, you must specify injection locations for liquid

droplet ammonia particles and set gaseous ammonia as the evaporation species. You must in-

clude this set of inputs in conjunction with the main ANSYS Fluent combustion calculation.

Since urea is a subliming solid, and usually is injected as a solution, mixed in water, you have

to define solid properties for urea under the Create/Edit Materials Dialog Box (p. ). It is assumed

that the water evaporates before urea begins its subliming process. The sublimation process is

modeled similar to the single rate devolatilization model of coal. You will supply the value for

the sublimation rate (s-). You must specify the water content while defining the injection

Specify the SNCR Reagent Species as nh3 (ammonia) or co<nh2> (urea) in the drop-down list.

When using the non-premixed combustion model with a liquid-phase reagent injection, enter a value

in the Reagent Fraction in Stream to specify the mass fraction of the reagent in the reagent stream.

The remaining mass fraction is assumed to be water. If you enabled a secondary stream in your PDF

calculation, by default the secondary stream will act as the reagent stream.You can assign the primary

stream as the reagent stream by using the text command that follows (enter  in response to the PDF

Stream ID prompt that follows the Injection Method prompt):

define/models/nox-parameters/nox-chemistry

If the Reagent Species selected is co <nh2> , then you will either accept the rate-limiting option

for Urea Decomposition, or specify the NH3 Conversion value when selecting a user-specified Urea

Decomposition.

You will use the urea decomposition under the SNCR tab to define which of the two decom-

position models is to be used. The first model (which is the default) is the rate-limiting decom-

position model, as given in Table . : Two-Step Urea Breakdown Process in the Theory Guide.

ANSYS Fluent will then calculate the source terms according to the rates given in Table . : Two-

Step Urea Breakdown Process in the Theory Guide. The second model is for when you assume

that the urea decomposes instantly into ammonia and HNCO at a given proportion. In this case,

you will specify the molar conversion fraction for ammonia, assuming that the rest of the urea

is converted to HNCO. An example value is given above.

The value for user-specified NH3 conversion is the mole fraction of NH3 in the mixture of NH3

and HNCO that is instantly created from the reagent injection. In this case, there is no urea

source because all of reagent is assumed to convert to both NH3 and HNCO, instantly.

.... Setting Turbulence Parameters

If you want to take into account turbulent fluctuations (as described in NOx Formation in Turbulent

Flows in the Theory Guide) when you compute the specified NOx formation (thermal, prompt, and/or

fuel, with or without reburn), define the turbulence parameters in the Turbulence Interaction Mode

tab.

Figure . : The NOx Model Dialog Box and the Turbulence Interaction Mode Tab

Select one of the options in the PDF Mode drop-down list in the Turbulence Interaction Mode tab:

tab.

Select temperature to take into account fluctuations of temperature.

Select temperature/species to take into account fluctuations of temperature and mass fraction of the

species selected in the Species drop-down list (which appears when you select this option).

(non-premixed and partially premixed combustion calculations only) Select mixture fraction to take into

account fluctuation in the mixture fraction(s).

Important

When modeling the formation of other pollutants along with NOx, you should compare

the selections made in the PDF Mode drop-down lists in the Turbulence Interaction

Mode group boxes of the NOx Model Dialog Box (p. ) and the Turbulence Interaction

Mode group boxes of the SOx Model and Soot Model dialog boxes. If mixture fraction

is selected in any of these dialog boxes, then it must be selected in all of the others as

well.

The mixture fraction option is available only if you are using either the non-premixed or partially

premixed combustion model to model the reacting system. If you use the mixture fraction option,

the instantaneous temperatures and species concentrations are taken from the PDF look-up table as

a function of mixture fraction and enthalpy and the instantaneous NOx rates are calculated at each

cell. The PDF used for convoluting the instantaneous NOx rates is the same as the one used to compute

the mean flow-field properties. For example, for single-mixture fraction models the beta PDF is used,

and for two-mixture fraction models, the beta or the double delta PDF can be used. The PDF for

mixture fraction is calculated from the values of mean mixture fraction and variance at each cell, and

the instantaneous NOx rates are convoluted with the mixture fraction PDF to yield the mean rates in

turbulent flow.

Note

When mixture fraction is selected as PDF mode, ANSYS Fluent calculates and tabu-

lates the NOx rates apriori for faster computations of NOx rates. The NOx rates are tabulated

at the first NOx iteration and a message

Performing Pollutant PDF integrations...

is displayed in the Fluent console.

If you selected temperature or temperature/species for the PDF Mode, you should define the fol-

lowing parameters in the Turbulence Interaction Mode tab:

PDF Type

allows you to specify the shape of the PDF, which is then integrated to obtain mean rates for the tem-

perature and (if you selected temperature/species for the PDF Mode) the species. If you select beta,

the PDF will be modeled using Equation . in the Theory Guide. If you select gaussian, the PDF will

be modeled using Equation . in the Theory Guide.

PDF Points

allows you to specify the number of points used to integrate the beta or Gaussian function in Equa-

tion . or Equation . in the Theory Guide on a histogram basis.The default value of  is a

minimum value. It is recommended that you run the calculation with this minimum value to convergence,

and then keep increasing the value (for example, –) until the pollutants of interest stop changing.

Increasing this value may improve accuracy, but will also increase the computation time.

Temperature Variance

allows you to specify the form of transport equation that is solved to calculate the temperature variance.

The default selection is algebraic, which is an approximate form of the transport equation (see Equa-

tion . of the Theory Guide).You also have the option of selecting transported to solve Equa-

tion . in the Theory Guide.Though the transported form is more exact, it is more expensive

computationally.

Tmax Option

provides various options for determining the maximum limit of the temperature used for the integration

of the PDF (see Equation . in the Fluent Theory Guide) to calculate mean rates for turbulent fluctuations

of NOx:

The default selection is global-tmax, which sets the limit as the maximum temperature in the flow

field.

You can select local-tmax if you would rather obtain cell-based maximum temperature limits by

multiplying the local cell mean temperature by the value entered in Tmax Factor.

You can select specified-tmax to set the limit for each cell to be the value entered in Tmax.

If you have selected a user-defined function in the NOx Rate drop-down list in the Formation tab,

then you can select user-defined so that the temperature limit is specified by a user-defined function.

Species

only appears if you have selected temperature/species for the PDF Mode.Your selection in this drop-

down menu determines which species’ mass fraction is included in the NOx formation calculations.

Important

Note that the species variance will always be calculated using the algebraic form of the

transport equation (Equation . in the Theory Guide).

Important

.... Defining Boundary Conditions for the NOx Model

At flow inlet boundaries, you must specify the Pollutant NO Mass Fraction, and if necessary, the

Pollutant HCN Mass Fraction, Pollutant NH3 Mass Fraction, and Pollutant N2O Mass Fraction.

Setup →

You can retain the default inlet values of zero for these quantities or you can enter nonzero numbers

as appropriate for your combustion system.

To solve for NOx products, perform the following steps:

. (optional) If the discrete phase model (DPM) is turned on (by enabling the Interaction with Continuous

Phase) to run with the NOx model, then set the DPM Iteration Interval to  such that no DPM iterations

are performed as the NOx case is being solved.

. In the Equations Dialog Box (p. ) of the Solution Controls Task Page (p. ), turn off the solution of all

variables except species NO (and HCN, NH3, or N2O, based on the model selected).

.

Solution →

. In the Solution Controls task page, set a suitable value for the NO (and HCN, NH3, or N2O, if appropriate)

under-relaxation. A value of . is suggested, although lower values may be required for certain problems

(that is, if convergence cannot be obtained, try a lower under-relaxation value).

. In the Residual Monitors Dialog Box (p. ), decrease the convergence criterion for NO (and HCN, NH3, or

N2O, if appropriate) to -.

Edit...

Edit...

residuals are below -) to ensure that the NO and HCN or NH3 concentration fields are no longer evolving.

Solution →

When you compute NOx formation, the following additional variables will be available for postprocessing:

Mass fraction of Pollutant no

Mass fraction of Pollutant hcn (appropriate fuel NOx model only)

Mass fraction of Pollutant nh3 (appropriate fuel NOx model only)

Mass fraction of Pollutant n2o (N2O-intermediate model only)

Mass fraction of Pollutant urea (SNCR urea injection)

Mass fraction of Pollutant hnco (SNCR urea injection)

Mass fraction of Pollutant nco (SNCR urea injection)

Mole fraction of Pollutant no

Mole fraction of Pollutant hcn (appropriate fuel NOx model only)

Mole fraction of Pollutant nh3 (appropriate fuel NOx model only)

Mole fraction of Pollutant n2o (N2O-intermediate model only)

Mole fraction of Pollutant urea (SNCR urea injection)

Mole fraction of Pollutant hnco (SNCR urea injection)

Mole fraction of Pollutant nco (SNCR urea injection)

no Density

hcn Density (appropriate fuel NOx model only)

nh3 Density (appropriate fuel NOx model only)

n2o Density (N2O-intermediate model only)

urea Density (SNCR urea injection)

hnco Density (SNCR urea injection)

nco Density (SNCR urea injection)

Rate of no (from the individual pathways)

Rate of hcn (appropriate fuel NOx model only)

Rate of nh3 (appropriate fuel NOx model only)

Rate of n2o (N2O-intermediate model only)

Rate of urea (SNCR urea injection)

Rate of hnco (SNCR urea injection)

Rate of nco (SNCR urea injection)

These variables are contained in the NOx... category of the variable selection drop-down list that appears

in postprocessing dialog boxes. Additional NO rates from individual pathways, Thermal, Prompt, Fuel,

N2O Path, and SNCR can be plotted.

The following sections describe how to use the SOx model in ANSYS Fluent. For information about the

theory behind the SOx models in ANSYS Fluent, see SOx Formation in the Theory Guide.

... Using the SOx Model

When the sulfur content in the fuel is low, SOx concentrations that are generated in combustion gen-

erally have minimal influence on the predicted flow field, temperature, and major combustion product

concentrations. The most efficient way to use the SOx model is as a postprocessor to the main com-

bustion calculation. However, if the sulfur content is high, then SOx formation should be coupled with

the gas phase combustion process rather than treating it as a postprocessing step.

The procedure for enabling and setting up the model for a decoupled solution is as follows:

. Calculate your combustion problem using ANSYS Fluent.

Important

The premixed combustion model and the Flamelet generated manifold model are not

compatible with the SOx model.

. Enable the SOx model, define the fuel streams, and set the appropriate parameters, as described in this

section.

Setup → Models → Species → SOx

Edit...

. Define the boundary conditions for SO2 and H2S (and SO3, SH, or SO if necessary) at flow inlets.

section.

Edit...

Setup →

. In the Equations Dialog Box (p. ), turn off the solution of all variables except species SO2 and H2S (and

SO3, SH, or SO, based on your selections).

Solution →

. Perform calculations until convergence (that is, until the SO2 and H2S—and SO3, SH, or SO, if

solved—species residuals are below -) to ensure that the SO2 and H2S concentration fields are no

longer evolving.

Solution →

. Review the mass fractions of SO2 and H2S (and SO3, SH, or SO) by generating graphical plots or alphanu-

meric reports in the usual way.

.... Enabling the SOx Model

To model SOx formation, enable the SOx Formation option in the SOx Model Dialog Box (p. )

(Figure . : The SOx Model Dialog Box (p. )).

Edit...

SOx Formation

Figure . : The SOx Model Dialog Box

When modeling fuel SOx formation, ANSYS Fluent allows you to define up to three separate fuel

streams, and to select the fuel  sources for each fuel stream.

Solid and liquid fuels (combusting particle and droplet) both contributing to fuel SOx.

Two or three solid fuels with different -content and SO2 /H2S production models (two or three

combusting particles), for example coal blends, coal-biomass cofiring, and so on.

Two or three liquid fuels with different -content and SO2 /H2S production models (two or three

droplet or multicomponent particles).

Gas and solid (or droplet) fuel both contributing to fuel SOx.

In addition, you can model one solid fuel contributing to SOx in the presence of another reacting

solid particle not containing any , by specifying the active  fuel source for SOx formation.

You can define multiple fuel streams when you are modeling SOx  formation, as shown in the following

steps:

. Specify the Number of Fuel Streams in the Fuel Streams group box.You are allowed up to three sep-

arate fuel streams.

a.

b. Select the Fuel Type in the Fuel Stream Settings group box.

c.

If your Fuel Type is Liquid or Solid, select the S sources from the Fuel Sources list.

in the SOx calculation.Your selection will be used to determine the char burnout rate

and

in Equation . and Equation . in the Theory Guide. Make sure

to deselect all combusting particle materials that do not contribute to SOx.

sources in the SOx calculation.Your selection will be used to determine the fuel release rate

in Equation . in the Theory Guide. Make sure to deselect all droplet and multicomponent

materials that do not contribute to SOx.

d. If the Fuel Type in your model is Gas, select one or more materials from the Fuel Species list.You

cannot select more than  fuel species for each fuel stream, and the total number of fuel species se-

lected for all the fuel streams combined cannot exceed .Your selection will be used to determine

the mean limiting reaction rate

e. Specify the parameters for this particular fuel stream in the Fuel Stream Settings group box. See

Defining the SOx Fuel Stream Settings (p. ) for details.

. Repeat steps . (a)–. (e) for each additional fuel stream.

Important

Important considerations should be made when reading case and data files set up in a

version of ANSYS Fluent . or earlier:

When reading a case and data file with multiple injection materials that was set up in a version

of ANSYS Fluent previous to and including ., ANSYS Fluent will initialize the injection ma-

terial specific fuel  sources for the fuel SOx model. ANSYS Fluent will perform a DPM iteration

when the flow iterations are initiated.

When reading a case file that was set up in a version older than ANSYS Fluent . with multiple

fuel streams defined for the SOx model, you must review the setup and select the S sources

from the Fuel Sources list.

.... Defining the SOx Fuel Stream Settings

When using the SOx model, you must set the parameters in the Fuel Stream Settings group box for

each fuel stream specified in the Fuel Stream ID field.

To calculate SOx formation from a solid fuel, select Solid under Fuel Type.

To calculate SOx formation from a liquid fuel, select Liquid under Fuel Type.

To calculate SOx formation from a gaseous fuel, select Gas under Fuel Type.

Figure . : The SOx Model Dialog Box Displaying Liquid Fuel Parameters

..... Setting SOx Parameters for Gaseous and Liquid Fuel Types

If you have selected Gas or Liquid as the Fuel Type, you must specify the following:

Select the intermediate species (h2s, so2, or h2s/so2) in the S Intermediate drop-down list.

Set the correct mass fraction of sulfur in the fuel (kg sulfur per kg fuel) in the Fuel S Mass Fraction field.

Specify the overall fraction of the fuel , by mass, that will be converted to the intermediate species

and/or product SO2 in the Conversion Fraction field.Therefore, any remaining  will not contribute to

SOx formation.This is based on the assumption that the remaining volatile  will convert to gas phase

sulfur.The Conversion Fraction for the S Intermediate has a default value of .

If you selected h2s/so2 as the intermediate, you must set the fraction of the converted fuel , by mass,

that will become h2s under Partition Fractions.The fraction of fuel  that will become SO2 will be cal-

culated by the remainder.

Note that setting a partition fraction of  for H2S is equivalent to assuming that all fuel S is con-

verted to the final product SO2.

..... Setting SOx Parameters for a Solid Fuel

For solid fuel, several inputs are required for the SOx model.

Figure . : The SOx Model Dialog Box Displaying Solid Fuel Parameters

Specify the mass fraction of sulfur in the volatiles in the Volatile S Mass Fraction field.

and/or product SO2 in the Conversion Fraction field.

If you selected h2s/so2 as the volatile  intermediate, you must specify the fraction of the converted

volatile , by mass, that will become h2s under Partition Fractions.The fraction of volatile  that will

become SO2 will be calculated by the remainder.

Select the char  conversion path from the Char S Conversion drop-down list as so2, h2s, or so2/h2s.

Specify the mass fraction of sulfur in the char in the Char S Mass Fraction field.

Specify the overall fraction of the char , by mass, that will be converted to the intermediate species

If you selected so2/h2s from the Char S Conversion drop-down list, you must specify the fraction of

the converted char , by mass, that will become SO2 under Partition Fractions.The fraction of char

that will become H2S will be calculated by the remainder.

The following equations are used to determine the mass fraction of sulfur in the volatiles and char:

(.)

where

= release rate of fuel sulfur in kg/s

= release rate of volatiles (v) or char (c) in kg/s

= mass fraction of sulfur in volatiles or char

Let

= total sulfur mass fraction in daf coal (that is, from daf ultimate analysis)

= char sulfur as a fraction of total sulfur

(.)

(.)

(.)

(.)

(.)

.... Defining the SOx Formation Model Parameters

You can set the SOx formation model parameters that apply to all of the fuel streams in the Formation

Model Parameters group box:

You have the option of including SO3 as a product, and including SH and SO as intermediates by enabling

the Include SO3 Product and the Include SH and SO Intermediates options, respectively. See Reaction

Mechanisms for Sulfur Oxidation in the Theory Guide for further information.

Specify the method by which O and OH will be calculated.The SOx routines employ three methods for

reduction calculations of SOx:

– You can select equilibrium, partial-equilibrium, or instantaneous in the [O] Model drop-down list.

– You can select none, partial-equilibrium, or instantaneous in the [OH] Model drop-down list.

Important

Important

To use the predicted O and/or OH concentration, select instantaneous in the [O]

Model or [OH] Model drop-down list.

If you want to take into account turbulent fluctuations when you compute the specified SO2 formation,

define the turbulence parameters in the Turbulence Interaction Mode group box.

Figure . : The SOx Model Dialog Box for a Gas Fuel Type with Turbulence

Select one of the options in the PDF Mode drop-down list:

Important

When modeling the formation of other pollutants along with SOx, you should compare

Mode tab of the NOx Model Dialog Box (p. ) and the Turbulence Interaction Mode

group boxes of the SOx Model and Soot Model dialog boxes. If mixture fraction is selected

in any of these dialog boxes, then it must be selected in all of the others as well.

a function of mixture fraction and enthalpy and the instantaneous SOx rates are calculated at each

cell. The PDF used for convoluting the instantaneous SOx rates is the same as the one used to compute

the instantaneous SOx rates are convoluted with the mixture fraction PDF to yield the mean rates in

lowing parameters in the Turbulence Interaction Mode group box:

PDF Type

PDF Points

tion . in the Theory Guide).You have the option of selecting transported to instead solve Equa-

tion . in the Theory Guide.Though the transported form is more exact, it is also more expensive

of SOx:

field.

If you have selected a user-defined function from the SOx Rate drop-down menu in the User-Defined

Functions group box, then you can select user-defined so that the limit is specified by a user-defined

function. See the Fluent Customization Manual for details about user-defined functions.

Species

down menu determines which species’ mass fraction is included in the SOx formation calculations.

Important

Important

.... Specifying a User-Defined Function for the SOx Rate

You can choose to specify a user-defined function for the rate of SOx production. By default, the rate

returned from the user-defined function is added to the rate returned from the standard SOx production

options. You also have the option of replacing ANSYS Fluent’s SOx rate calculations with your own

user-defined SOx rate.

In addition to or instead of using the UDF to specify the SOx rate, you can use it to specify custom

To use a UDF to add a rate to ANSYS Fluent’s SOx rate calculations, you must compile and load the

desired function, and then select it from the SOx Rate drop-down list in the User-Defined Functions

group box. After you have selected the UDF, you have the following options:

You can specify that your custom rate is added to the ANSYS Fluent SOx rate calculations, by retaining

the default selection of Add to the Fluent Rate in the UDF Rate group box.

You can replace the ANSYS Fluent SOx rate calculations with your custom rate, by selecting Replace Fluent

Rate in the UDF Rate group box.

list in the Turbulence Interaction Mode group box.

.... Defining Boundary Conditions for the SOx Model

At flow inlet boundaries, you must specify the Pollutant SO Mass Fraction, and if necessary, the

Pollutant SH Mass Fraction, Pollutant H2S Mass Fraction, Pollutant SO3 Mass Fraction, and Pol-

lutant SO2 Mass Fraction in the Species tab, as demonstrated in Figure . : The Mass-Flow Inlet

Dialog Box: the Species Tab (p. ).

Setup →

Figure . : The Mass-Flow Inlet Dialog Box: the Species Tab

To solve for SOx products:

(optional) If the discrete phase model (DPM) is turned on (by enabling the Interaction with Continuous

Phase) to run with the SOx model, then set the DPM Iteration Interval to  such that no DPM iterations

are performed as the SOx case is being solved.

In the Equations Dialog Box (p. ) of the Solution Controls Task Page (p. ), turn off the solution of all

variables except Pollutant so2 and Pollutanth2s (and Pollutant so3, Pollutant sh, and Pollutant so, if

applicable).

Solution →

In the Solution Controls Task Page (p. ), set suitable values for the pollutant SO2 and H2S (and SO3, SH,

and SO, if applicable) under-relaxation factors. A value of . is suggested, although lower values may be

required for certain problems.That is, if convergence cannot be obtained, try a lower under-relaxation

value.

Solution →

Controls

value.

Solution →

Controls

Under Spatial Discretization in the Solution Methods Task Page (p. ), select the desired scheme for

each of the pollutants, SO2 and H2S (and SO3, SH, and SO, if applicable)

Solution →

Methods

In the Residual Monitors Dialog Box (p. ), decrease the convergence criterion for the pollutants SO2 and

H2S (and SO3, SH, and SO, if applicable) to -.

Edit...

Perform calculations until convergence (that is, until the SO2 and H2S—and SO3, SH, and SO—pollutant

residuals are below -) to ensure that SO2 and H2S (and SO3, SH, and SO) concentration fields are no

Solution →

Review the mass fractions of pollutants, SO2 and H2S (and SO3, SH, and SO), by generating graphical plots

or alphanumeric reports as described in Postprocessing (p. ).

When you compute SOx formation, the following additional variables will be available for postprocessing.

They are contained in the SOx... category of the variable selection drop-down list that appears in

postprocessing dialog boxes.

Mass fraction of pollutant so2

Mass fraction of pollutant h2s

Mass fraction of pollutant so3

Mass fraction of pollutant sh

Mass fraction of pollutant so

Mole fraction of pollutant so2

Mole fraction of pollutant h2s

Mole fraction of pollutant so3

Mole fraction of pollutant sh

Mole fraction of pollutant so

so2 Density

h2s Density

so3 Density

sh Density

so Density

Rate of so2

Rate of h2s

Rate of so3

Rate of sh

Rate of so

sh Density

so Density

Rate of so2

Rate of h2s

Rate of so3

Rate of sh

Rate of so

This section contains information about using the soot formation models in ANSYS Fluent. For inform-

ation about the theory behind the soot models in ANSYS Fluent, see Soot Formation in the Theory

Guide.

... Using the Soot Models

When the mass fraction of soot is relatively large (for example, %) or if your problem involves the

effect of radiation, the soot formation should be computed as part of the main combustion solution

and not through postprocessing (as is done for the NOx and SOx models). The procedure for setting

up and solving a soot formation model is outlined below. Only the steps that are pertinent to soot

conjunction with the soot formation model, see the appropriate sections for those models.

. Set up your combustion problem using ANSYS Fluent as usual. Note the following limitations:

None of the soot models are compatible with premixed combustion.

The one-step and two-step soot formation models are only available for turbulent flows.

. Enable the desired soot formation model and set the related parameters, as described in this section.

Setup → Models → Species → Soot

Edit...

. Define the boundary conditions for soot (and nuclei, if you are not using the one-step model) at flow inlets.

Setup →

. In the Solution Controls Task Page (p. ), set a suitable value for the soot (and nuclei, if you are not using

Setup →

the one-step model) under-relaxation factor(s).The default value is .. If convergence cannot be obtained

with this value, try a lower under-relaxation value.

Solution →

Controls

. Perform calculations until convergence (that is, until the soot / nuclei residual is below -) to ensure

that the soot (and nuclei) field is no longer evolving.

Solution →

Note that when Soot-Radiation Interaction is enabled in the Soot Model dialog box, soot equations

(soot, nuclei, and tar species, if available) must be solved together with the combustion solution

to obtain correct radiation coupling. Therefore, when Soot-Radiation Interaction is enabled, the

soot equations are not available for pollutant postprocessing, but will be solved together with the

combustion solution. However, if other pollutants are to be solved (while soot/radiation interaction

is enabled), those pollutant equations can be postprocessed.

. Review the mass fraction of soot (and nuclei) by generating graphical plots or alphanumeric reports in

the usual way.

.... Setting Up the One-Step Model

You can enable and set up the one-step soot formation model by using the Soot Model Dialog

Box (p. ) (Figure . : The Soot Model Dialog Box for the One-Step Model (p. )).

Edit...

Soot Formation

Figure . : The Soot Model Dialog Box for the One-Step Model

. Under Model, select One-Step.The dialog box will expand to show the appropriate inputs.

Edit...

. Define the fuel and oxidizer species. Under Species Definition, select the fuel in the Fuel drop-down

list and the oxidizer in the Oxidant drop-down list. If you are using the non-premixed model for the

combustion calculation and your fuel stream consists of a mixture of components, you should choose

the most appropriate species as the Fuel species for the soot formation model. Similarly, the most signi-

ficant oxidizing component (for example, O2) should be selected as the Oxidant.

. If you want to include the effects of soot formation on the radiation absorption coefficient, enable Soot-

Radiation Interaction in the Options group box. For more details, see The Effect of Soot on the Absorp-

tion Coefficient in the Theory Guide.

. Define the following Process Parameters:

Stoichiometry for Soot Combustion

is the mass stoichiometry,

, in Equation . in the Theory Guide, which computes the soot

combustion rate.The default value of . assumes that the soot is pure carbon and the oxidizer

is O2.

Stoichiometry for Fuel Combustion

combustion rate.The default value supplied by ANSYS Fluent (.) is for combustion of propane

(C3H8) by oxygen (O2).

. Set the Modeling Parameters that are used in Equation ., Equation ., and Equation .

in the Theory Guide:

Soot Formation Constant

(kg/n-m-s) in Equation . in the Theory Guide.

Equivalence Ratio Exponent

is the exponent  in Equation . in the Theory Guide.

Equivalence Ratio Minimum

and Equivalence Ratio Maximum are the minimum and maximum values of the fuel equivalence

ratio  in Equation . in the Theory Guide.This equation will be solved only if Equivalence Ratio

Minimum

Equivalence Ratio Maximum; if  falls outside of this range, it is assumed that soot

does not form.

Activation Temperature of Soot Formation Rate

is the term

Magnussen Constant for Soot Combustion

is the constant  used in the rate expressions governing the soot combustion rate (Equation .

and Equation . in the Theory Guide).

Note that the default values for these parameters are for propane fuel [] (p. ), [] (p. ), which

are valid for a wide range of hydrocarbon fuels.

.... Setting Up the Two-Step Model

You can enable and set up the two-step soot formation model by using the Soot Model Dialog

Box (p. ) (Figure . : The Soot Model Dialog Box for the Two-Step Model (p. )).

Edit...

Figure . : The Soot Model Dialog Box for the Two-Step Model

. Under Model, select Two-Step.The dialog box will expand to show the appropriate inputs.

Important

Note that the two-step Tesner model should only be used when the eddy-dissipation

model is used to define the turbulence-chemistry interaction.

. Under Species Definition, select the fuel in the Fuel drop-down list and the oxidizer in the Oxidant

drop-down list. If you are using the non-premixed model for the combustion calculation and your fuel

stream consists of a mixture of components, you should choose the most appropriate species as the

Fuel species for the soot formation model. Similarly, the most significant oxidizing component (for ex-

ample, O2) should be selected as the Oxidant.

Mean Diameter of Soot Particle, Mean Density of Soot Particle

are the assumed average diameter and average density of the soot particles in the combustion system,

used to compute the soot particle mass

in Equation . in the Theory Guide . Note that the

default values for soot density and diameter are taken from [] (p. ).

is the mass stoichiometry

in Equation . in the Theory Guide, which computes the soot

is O2.

(

) by oxygen (

).

. Set the Modeling Parameters that are used in Equation ., Equation ., Equation .,

Equation ., and Equation . in the Theory Guide:

Limiting Nuclei Formation Rate

is the limiting value of the kinetic nuclei formation rate,

Below this limiting value, the branching and termination term, (

) in Equation . in the Theory

Guide, is not included.

Nuclei Branching-Termination Coefficient

is the term

Nuclei Coefficient of Linear Termination on Soot

is the term

Pre-Exponential Constant of Nuclei Formation

is the pre-exponential term

in the kinetic nuclei formation term, Equation . in the Theory

Guide.

Activation Temperature of Nuclei Formation Rate

is the term

in the kinetic nuclei formation term, Equation . in the Theory Guide.

Alpha for Soot Formation Rate

is , the constant in the soot formation rate equation, Equation . in the Theory Guide.

Beta for Soot Formation Rate

Magnussen Constant for Soot and Nuclei Combustion

The default values for the two-step model are the same as in Magnussen and Hjertager [] (p. )

(for acetylene flame), except for

, which is assumed to have the original value from Tesner et

al. [] (p. ). If your model involves propane fuel rather than acetylene,

= .5x108 [] (p. ) is

recommended. For best results, you should modify both of these parameters using empirically de-

termined inputs for your specific combustion system.

.... Setting Up the Moss-Brookes Model and the Hall Extension

You can enable and set up the Moss-Brookes and Moss-Brookes-Hall soot formation models by using

the Soot Model Dialog Box (p. ) (Figure . : The Soot Model Dialog Box for the Moss-Brookes

Edit...

Figure . : The Soot Model Dialog Box for the Moss-Brookes Model

. Under Model, select Moss-Brookes or Moss-Brookes-Hall.The dialog box will expand to show the ap-

propriate inputs. Note the following about these models:

The Moss-Brookes model was originally proposed for soot prediction in methane flames. However,

it can be equally applicable to higher hydrocarbon species by appropriately modifying the soot pre-

cursor and participating surface growth species.

The Moss-Brookes-Hall model is applicable for higher hydrocarbon fuels (for example, kerosene) and

will only be available when C2H2, C6H6, C6H5, and H2 are present in the gas phase species list.

. Define the precursor species in the Species Definition group box.When suitable precursor species are

present in the species list, you can select species-list from the Precursor from drop-down list, and then

select the Soot Precursor species and the Surface Growth species from the selection lists. Note that

for the Moss-Brookes model, you can select acetylene (c2h2), ethylene (c2h4), and/or benzene (c6h6)

for the Soot Precursor; if neither are present or if you would like to specify a different precursor correl-

ation, then curve fitting will be used to determine the precursor and surface growth species mass fractions

(see Species Definition for the Moss-Brookes Model with a User-Defined Precursor Correlation (p. ) for

further details regarding curve fitting).

. Specify how turbulent fluctuations will be accounted for in the soot formation calculations by defining

the turbulence parameters in the Turbulence Interaction Mode group box. Select one of the options

in the PDF Mode drop-down list:

Select none to ignore turbulence and use laminar soot rate calculations.

Select temperature/species to take into account fluctuations of temperature and mass fraction of

the species selected in the Species drop-down list (which appears when you select this option).

(non-premixed and partially premixed combustion calculations only) Select mixture fraction to take

into account fluctuation in the mixture fraction(s).This is the recommended approach, as it generally

yields the best results and accuracy.

Important

When modeling the formation of other pollutants along with soot, you should compare

group boxes of the SOx Model and Soot Model dialog boxes. If mixture fraction is

selected in any of these dialog boxes, then it must be selected in all of the others as

well.

the instantaneous temperatures and species concentrations are taken from the PDF look-up table

as a function of mixture fraction and enthalpy and the instantaneous soot production rates are

calculated at each cell. The PDF used for convoluting the instantaneous soot rates is the same as

the one used to compute the mean flow-field properties. For example, for single-mixture fraction

models the beta PDF is used, and for two-mixture fraction models, the beta or the double delta

PDF can be used. The PDF in terms of mixture fraction is calculated from the values of mean

mixture fraction and variance at each cell, and the instantaneous soot rates are convoluted with

the mixture fraction PDF to yield the mean rates in turbulent flow.

Note

When mixture fraction is selected as PDF mode, ANSYS Fluent calculates and tabulates

the soot rates apriori for faster computations of soot rates. The soot rates are tabulated

at the first soot iteration and a message

. If you selected temperature or temperature/species for the PDF Mode, you should define the following

parameters in the Turbulence Interaction Mode group box:

PDF Type

allows you to specify the shape of the PDF, which is then integrated to obtain mean rates for the

temperature and (if you selected temperature/species for the PDF Mode) the species. If you select

beta, the PDF will be modeled using Equation . in the Theory Guide. If you select gaussian,

the PDF will be modeled using Equation . in the Theory Guide.

PDF Points

tion . or Equation . in the Theory Guide on a histogram basis.The default value of  is

a minimum value. It is recommended that you run the calculation with this minimum value to con-

vergence, and then keep increasing the value (for example, –) until the pollutants of interest

stop changing. Increasing this value may improve accuracy, but will also increase the computation

time.

allows you to specify the form of transport equation that is solved to calculate the temperature

variance.The default selection is algebraic, which is an approximate form of the transport equation

(see Equation . of the Theory Guide).You have the option of selecting transported to instead

solve Equation . in the Theory Guide.Though the transported form is more exact, it is also

more expensive computationally.

provides various options for determining the maximum limit of the temperature used for the integ-

ration of the PDF (see Equation . in the Fluent Theory Guide) to calculate mean rates for turbulent

fluctuations of soot.The default selection is global-tmax, which sets the limit as the maximum

temperature in the flow field.You can select local-tmax if you would rather obtain cell-based max-

imum temperature limits by multiplying the local cell mean temperature by the value entered in

Tmax Factor.You can select specified-tmax to set the limit for each cell to be the value entered in

Tmax. Finally, if you have compiled a user-defined function for the soot rate and loaded the library

into ANSYS Fluent, then you can select user-defined so that the limit is specified by a user-defined

function.

Species

only appears if you have selected temperature/species for the PDF Mode.Your selection in this

function.

Species

drop-down menu determines which species’ mass fraction is included in the soot formation calcula-

tions.

Important

Note that the species variance will always be calculated using the algebraic form of

the transport equation (Equation . in the Theory Guide).

. Under Process Parameters, enter information about the mass and mean density of the soot particles:

Mass of Incipient Soot Particles

is

in Equation . and Equation . in the Theory Guide. Note that this value was assumed

to be  kg/kmol ( carbon atoms) in the work of Brookes and Moss, whereas the Hall extension

model assumed it to be  kg/kmol ( carbon atoms).

Mean Density of Soot Particle

is

to be  kg/m3 in the work of Brookes and Moss [] (p. ), whereas Hall et al. [] (p. ) assumed

it to be  kg/m3.

. Select the Soot Oxidation Model.Your choices include the Fenimore-Jones model, as originally used

in Brookes and Moss’ work, or the Lee extended model.The Lee model will model soot oxidation due

to hydroxyl radicals as in the Fenimore-Jones model, as well as the oxidation due to molecular oxygen.

. Set the Modeling Parameters:

[OH] Model

allows you to specify the method by which the OH radical concentration is calculated.The recom-

mended selection from the drop-down list is instantaneous, although this option is only available

when OH is available in the species list and is calculated by the combustion model.The other option

is the partial-equilibrium model, which necessitates the availability of O radical concentration

within the field.

[O] Model

[O] Model

must be defined when you have selected partial-equilibrium for the [OH] Model, and specifies the

method by which the O radical concentration is calculated.The options include equilibrium, partial-

equilibrium, and instantaneous.

Note that in ANSYS Fluent, the oxidation rate scaling parameter (

Guide) is set to unity. If you would like to change the value of this parameter, you can use the

define/models/soot-parameters text command. A lower value will reduce the amount of

soot oxidation.

..... Specifying a User-Defined Function for the Soot Oxidation Rate

You can choose to specify a user-defined function for the soot oxidation rate. The compiled UDF

hook is available from the User Defined Oxidation Rate drop-down list of the Soot Model dialog

box. See DEFINE_SOOT_OXIDATION_RATE in the Fluent Customization Manual for details about

user-defined functions.

..... Specifying a User-Defined Function for the Soot Precursor Concentration

hook is available from the User Defined Precursor drop-down list in the Species Definition group

box of the Soot Model dialog box. See DEFINE_SOOT_PRECURSOR in the Fluent Customization

..... Species Definition for the Moss-Brookes Model with a User-Defined Precursor

Correlation

ANSYS Fluent accepts the following as possible precursor species for the Moss-Brookes model: C2H2,

C6H6, and C2H4. If none of these species are present in the species list (as is often the case when

using the eddy-dissipation model) or if you would prefer to specify a different precursor correlation,

your setup for the Moss-Brookes model will be different than noted previously. Under such circum-

stances, you should select user-correlation from the Precursor from drop-down list in the Species

Definition group box (note that this is only option possible when the appropriate species are not

present). The Soot Model Dialog Box (p. ) will then be as shown in Figure . : The Soot Model

Dialog Box for the Moss-Brookes Model with a User-Defined Precursor Correlation (p. ). The para-

meters you set in the Species Definition group box allow ANSYS Fluent to calculate a mixture

fraction based on the mass fractions of the oxidant and the carbon/hydrogen contributed by a

designated fuel species. The precursor species mass fraction will then be computed as a function

(which you will also define) of this mixture fraction.

Figure . : The Soot Model Dialog Box for the Moss-Brookes Model with a User-Defined

Precursor Correlation

. In the Species Definition group box, select a Fuel species and enter the related Fuel Carbon Number

and Fuel Hydrogen Number for use in the mixture fraction calculation.

. Enter the Molecular Weight of Precursor (the default value is for acetylene).

. Make a selection in the Precursor Correlation drop-down list to indicate how the precursor mass

fraction will be related to the mixture fraction. A piecewise-polynomial profile is defined by default.

Important

Note that the default values for the piecewise-polynomial profile are only valid for

a methane diffusion flame simulation, in which both the air and fuel initial temperatures

are set to  K, and acetylene is assumed as the soot precursor.

If you decide not to use the default values for Precursor Correlation, define the correlation

between the precursor mass fraction and the mixture fraction. This correlation should be based

on a laminar flamelet profile that you have generated. If possible, you should generate the profile

using the Species Model dialog box (as described in Setting Up the Steady and Unsteady Diffusion

Flamelet Models (p. )) with Steady Flamelet selected in the Chemistry tab. If there is no

mechanism, you can generate the profile using the equilibrium chemistry model (see Setting Up

the Equilibrium Chemistry Model (p. ) for details). You may also use a third-party software

package of your choice. You should then apply a curve-fitting technique to your generated profile,

to obtain either a constant value or a piecewise-polynomial function.

In a piecewise-polynomial function, the laminar flamelet profile is divided into a number of

mixture fraction ranges. In each range, the precursor species mass fraction

is defined using

the following equation:

(.)

where

is the number of coefficients , and  is the mixture fraction. The following piecewise-

polynomial function corresponds to the default settings in ANSYS Fluent:

(.)

(.)

where

(.)

. To define a piecewise-polynomial profile to relate the precursor mass fraction to the mixture

fraction, select piecewise-polynomial from the Precursor Correlation drop-down list and click

the Edit... button.

In the Piecewise-Polynomial Profile Piecewise-Polynomial Profile Dialog Box (p. ), set the

following controls:

a.

Enter the number of Ranges. For the example shown in Equation . (p. ), three ranges of

mixture fraction are defined, which is the maximum allowed.

b. For the first range (Range = ), enter the Minimum and Maximum mixture fraction values, and the

number of Coefficients. (Up to eight coefficients are available.) The number of coefficients defines

the order of the polynomial. An input of  defines a polynomial of order , and the mass fraction

will be constant and equal to the single coefficient. An input of  defines a polynomial of order ,

and the mass fraction will vary linearly with mixture fraction, and so on.

c.

Define the values for the coefficients in the Coefficients group box.The dialog box in Fig-

ure . :The Piecewise-Polynomial Profile Dialog Box (p. ) shows the inputs for the first range

d. Increase the value of Range and enter the Minimum and Maximum mixture fractions, number of

Coefficients, and the values for the Coefficients for the next range. Repeat if there is a third range.

Important

Note when defining the ranges, you must start with the lowest mixture fraction

range, and then proceed in order to the highest range. The solver will not sort

Important

them for you.

. To define a constant profile to relate the precursor mass fraction to the mixture fraction, select constant

from the Precursor Correlation drop-down list and enter a value in the accompanying text entry box.

.... Setting Up the Method of Moments Soot Model

You can enable and set up the Method of Moments model by using the Soot Model dialog box

(Figure . : The Soot Model Dialog Box for the Method of Moments Model (p. )).

Edit...

. In the Soot Model dialog box under Model, select Method of Moments.The dialog box will expand to

show the appropriate inputs.

Figure . : The Soot Model Dialog Box for the Method of Moments Model

. Specify Number Of Moments.

ANSYS Fluent will solve an equal number of moment transport equations. The default value of

moments works reasonably well for a wide range of applications. However, you can specify up to

moments to achieve higher accuracy.

. From the Soot Mechanism group box, select an appropriate option to use for soot modeling:

Detailed CHEMKIN Format: allows you to use a soot mechanism in CHEMKIN format. See Detailed

Soot Mechanism in the Fluent Theory Guide for details about this option.

Built-In HACA: allows you to set up the nucleation mechanism and use the-built-in HACA surface

growth and oxidations mechanisms. See Built-In HACA Mechanism in the Fluent Theory Guide for details

about this option.

. If you selected Detailed CHEMKIN Format, perform the following steps:

Figure . : The Soot Model Dialog Box for the Detailed CHEMKIN Format Soot Mechanism

a.

Under Process Parameters, specify Normalization Parameter for Moments.

The normalization parameter is used to minimize numerical errors when solving the normalized

soot moment transport equations. The default value for this parameter is enough for most

cases.

b. Prior to using this model, you must import the soot mechanism in a CHEMKIN format through the

File menu:

In the Import CHEMKIN Format Mechanism dialog box that opens, select the Import Surface

Mechanism option and provide a full pathname to the kinetics input file under the Surface

group box.

For more information about importing soot mechanisms, see Importing a Surface Kinetic

Mechanism in CHEMKIN Format (p. ).

. If you selected Built-In HACA (as shown in Figure . :The Soot Model Dialog Box for the Method of

Moments Model (p. )), perform the following steps:

a.

From the Soot Nucleation Model group box, select one of the following options:

Use Precursor (default): Enables you to define the precursor species for your soot prediction sim-

ulation.

Specify Mechanism: Enables you to provide the nucleation rate and specify nucleation as a reaction

between soot precursors. Using this option, you can achieve more accurate results where the

nucleation rate data is available.

b. (if Use Precursor is selected for the soot nucleation model) Under the Species Definition group

box, define precursor species.

i.

In the Soot Precursor group list (which is populated with all precursors available in your analysis),

select one or more precursors.

i.

The soot precursor species must be a hydrocarbon species. ANSYS Fluent uses kinetic

theory to calculate the nucleation rates considering coagulation between precursor species.

ii.

Click Sticking Coefficients... to specify the sticking coefficient for each precursor in the Sticking

Coefficients dialog box that will open.

Figure . : Sticking Coefficients for Soot Precursors

You must specify the sticking coefficient for each precursor because the nucleation rates

calculated based on kinetic theory of collision of two soot precursors are generally very

large, causing numerical errors.

Important

The default value for a sticking coefficient is calculated based on precursor

molecular weight. In general, you can use smaller values for sticking coefficients

for smaller precursors. For guidelines on specifying the sticking coefficients for

precursor species, see Nucleation in the Fluent Theory Guide.

c.

(if Specify Mechanism is selected for the soot nucleation model) Click Set Nucleation Mechanism...

and enter the reaction rates inputs in the Mechanism dialog box that will open.

Figure . : Settings for the Nucleation Mechanism

i.

Specify Number of nucleation reactions.

The nucleation reactions can be single or multi-step.

ii.

For each reaction, specify the following:

Reactant species and corresponding stoichiometric coefficient and rate exponent

The Arhenius Rate parameters (Pre-Exponential Factor, Activation Energy, and Temperature

Exponent)

Note

The inputs in the Mechanism dialog box are required only for reactant species as

Exponent)

Note

the main product of specified nucleation reaction is always assumed to be a soot

nuclei, and all other products are not considered in calculations of soot nucleation

rates.

d. If you want to account for soot aggregate formation, select Enable Aggregation Model

In addition to the moment transport equations, ANSYS Fluent will solve an equal number of

the particle moment transport equations.

Once you have enabled the aggregation model, you can specify the following parameters:

Critical diameter: A value of the soot particle diameter above which the coagulation regime

is switched from coalescent coagulation to aggregate coagulation.

Fractal Dimension: A parameter that describes the fractal structure of the aggregate. Values

between . and . work reasonably good for the aggregate coagulation.

Note

When the Enable Aggregation Model option is enabled, the Method of Mo-

ments model tends to over-predict the production of soot. This is due, in part,

to the linear interpolation of the particle moments. This aspect of the over-

prediction can be overcome by employing quadratic interpolation of the particle

moments. Another reason for the over-prediction of soot is due to how ANSYS

Fluent currently ignores the depletion of acetylene during the soot calculations.

Acetylene is consumed during the surface growth of soot, and since the gas

field stays frozen and has no knowledge of the soot process, thereby producing

a higher surface growth of soot, and eventually higher soot yields.

For information about the aggregation model, see Soot Aggregation in the Fluent Theory Guide.

e. Under Soot Surface Growth Options, specify Soot Density.

The growth of soot due to surface reactions and depletion due to oxidation reactions are

modeled using HACA mechanism (see Surface Growth and Oxidation in the separate Theory

Guide). For reaction rates and reaction steps, ANSYS Fluent uses default values and requires

no user inputs except for the soot site density.

Note

You can specify and/or edit the reaction rates of surface reactions using the

define/models/soot-parameters text command.

Important

The soot site density is always provided in units of number of sites per cm2 irrespect-

ive of the unit system selected in ANSYS Fluent.

f.

Under Process Parameters, specify Mean Density of Soot Particle and Normalization Parameter

for Moments.

soot moment transport equations. The default value for this parameter is sufficient, and you

may not need to change it.

g. Specify the Modeling Parameters:

[OH] Model: Specifies the method by which the [OH] radical concentration is calculated. For OH

Model, the following options are available:

– instantaneous (recommended where possible)

This option is only available when OH is present in the species list and participate in the

combustion simulation.

– partial-equilibrium

This option necessitates the availability of [O] atom concentration within the field.

[O] Model (available only if instantaneous is not selected for OH Model): Specifies the method

by which the [O] radical concentration is calculated.The following options are available:

– equilibrium

– instantaneous

.... Defining Boundary Conditions for the Soot Model

At flow inlet boundaries, you must specify the Soot Mass Fraction and (when not using the one-step

model) the Nuclei mass concentration. These correspond to

in Equation . and Equa-

tion . and

in Equation . and Equation . in the Theory Guide, respectively.

Setup →

You can retain the default inlet values of zero for both quantities or you can enter nonzero numbers

.... Reporting Soot Quantities

ANSYS Fluent provides additional reporting options when your model includes soot formation. You

Mass fraction of Soot

Mole fraction of Soot

Soot Density

Soot Volume fraction

Rate of Soot

Normalized Concentration of Nuclei (unavailable for one-step model)

Rate of Nuclei (unavailable for one-step model)

Rate of Soot Mass Nucleation (Moss-Brookes and Moss-Brookes-Hall models only)

Rate of Surface Growth (Moss-Brookes and Moss-Brookes-Hall models only)

Rate of Oxidation (Moss-Brookes and Moss-Brookes-Hall models only)

Rate of Nucleation (Moss-Brookes and Moss-Brookes-Hall models only)

Rate of Coagulation (Moss-Brookes and Moss-Brookes-Hall models only)

Soot Surface Area (Method of Moments model only)

Soot Mean Diameter (Method of Moments model only)

Concentration of soot species-n  (Method of Moments model only)

Site fraction of soot species-n  (Method of Moments model only)

Normalized soot moments (Method of Moments model only)

Normalized Soot Aggregation Moments (Method of Moments model with Aggregation only)

Average Number of Particles in Soot Aggregate (Method of Moments model with Aggregation only)

Primary Particle Diameter (Method of Moments model with Aggregation only)

These parameters are contained in the Soot... category of the variable selection drop-down list that

The decoupled detailed chemistry pollutant model is used to postprocess slowly-forming, trace pollutant

species on a steady-state flow field using detailed chemical kinetic mechanisms. For theoretical inform-

ation, refer to Decoupled Detailed Chemistry Model. The recommended procedure is as follows:

. Calculate your steady combustion problem using the Species Transport, Non-Premixed, Partially-Premixed,

or PDF Transport models in ANSYS Fluent. It is recommended that you save your case and data file, as it

may be difficult to revert to the original settings after you set up the decoupled detailed chemistry pollutant

model.

. Enable the Decoupled Detailed Chemistry option in the Decoupled Detailed Chemistry dialog box.To

access this dialog box, make sure that either the non-premixed or partially premixed model is selected, or

that reactions are enabled if the species transport or PDF transport models are used.

Setup → Models → Species → Decoupled Detailed Chemistry

Edit...

Figure . : The Decoupled Detailed Chemistry Dialog Box

Edit...

Using the Decoupled Detailed Chemistry Model

. Click Import CHEMKIN Mechanism... to import your detailed chemistry mechanism in CHEMKIN format.

The Import CHEMKIN Format Mechanism dialog box (described in Importing a Volumetric Kinetic

Mechanism in CHEMKIN Format (p. )) will open, where you will browse to the file. After the CHEMKIN

mechanism is imported, the Decoupled Detailed Chemistry dialog box will expand to include the species.

The species in the initial detailed chemical kinetic mechanism used to obtain the steady-state solution

appear in the Original Species list. The species in the detailed chemistry mechanism you have im-

ported appear in the Pollutant Species list. Note that if the species is present in both mechanisms,

it will be listed only under Original Species and will not be available as a pollutant species.

. Select the Pollutant Species and click Apply.The pollutant species are typically slowly forming (far from

chemical equilibrium), and occur at miniscule mass fractions. ANSYS Fluent will create a mixture material

called pollutant-mixture and enable the Species Transport model with the Stiff Chemistry Solver. All

species in the imported mechanism that were not in the original combustion model and are not pollutant

species will be calculated by chemical equilibrium at the cell temperature.The solution of all transport

equations, except the selected pollutant species, are disabled.

Note

Species that are not identified as pollutants and do not participate in the reactions

amongst the pollutant species are eliminated. Similarly, reactions in the imported CHEMKIN

Note

mechanism, which do not include any pollutant species are also eliminated.

. Click Integration Parameters... to open the Integration Parameters dialog box. Set the ISAT Parameters,

such as the ISAT Error Tolerance and Max. Storage. An ISAT Error Tolerance of 1e- is recommended,

and Max. Storage should be set to a large fraction of the free RAM memory available.To learn more about

setting integration parameters, refer to Using ISAT (p. ).

. Define the boundary conditions for all pollutants at flow inlets (these are usually zero).

Setup →

. Iterate until convergence.

Solution →

. Review the mass fractions of pollutants by generating graphical plots or alphanumeric reports in the usual

way.

Chapter : Predicting Aerodynamically Generated Noise

This chapter provides an overview of ANSYS Fluent’s approaches to computing aerodynamically generated

sound, the model setup, and the procedure for computing sound. For more information about the un-

derlying theory behind aerodynamically generated sound, see Aerodynamically Generated Noise in the

.. Using the Ffowcs Williams and Hawkings Acoustics Model

.. Using the Acoustics Wave Equation Model

.. Using the Broadband Noise Source Models

Considering the breadth of the discipline and the challenges encountered in aerodynamically generated

noise, it is not surprising that a number of computational approaches have been proposed over the

years whose sophistication, applicability, and cost widely vary.

ANSYS Fluent offers three approaches to computing aerodynamically generated noise: a direct approach,

a hybrid approach, and an approach that utilizes broadband noise source models. Within the hybrid

approach, Fluent offers the two methods, which are the integral method by Ffowcs Williams and

Hawkings, and a differential sound propagation method based on a finite volume solver for a wave

equation.

... Direct Method

... Integral Method by Ffowcs Williams and Hawkings

... Method Based on Wave Equation

... Broadband Noise Source Models

In this method, both generation and propagation of sound waves are directly computed by solving

the appropriate fluid dynamics equations. Prediction of sound waves always requires time-accurate

solutions to the governing equations. Furthermore, in most practical applications of the direct method,

one has to employ governing equations that are capable of modeling viscous and turbulence effects,

such as unsteady Navier-Stokes equations (that is, DNS), RANS equations, and filtered equations used

in LES and hybrid RANS-LES models.

The direct method is therefore computationally difficult and expensive inasmuch as it requires highly

accurate numerics, very fine computational meshes all the way to receivers, and acoustically nonreflect-

ing boundary conditions. The computational cost becomes prohibitive when sound is to be predicted

in the far field (for example, hundreds of chord-lengths in the case of an airfoil). The direct method

becomes feasible when receivers are in the near field (for example, cabin noise). In many such situations

involving near-field sound, sounds (or pseudo-sounds for that matter) are predominantly due to local

hydrodynamic pressure, which can be predicted with a reasonable cost and accuracy.

Since sound propagation is directly resolved in this method, you would normally solve the compressible

form of the governing equations (for example, compressible RANS equations, compressible form of

filtered equations for LES). Only in situations where the flow is low subsonic and the receivers in the

near field sense primarily local hydrodynamic pressure fluctuations (that is, pseudo sound) can incom-

pressible flow formulations be used. But this incompressible treatment will also not allow you to sim-

ulate resonance and feedback phenomena.

For predictions of mid- to far-field noise, the methods based on Lighthill’s acoustic analogy  [] (p. )

offer viable alternatives to the direct method. In this approach, the near-field flow obtained from ap-

propriate governing equations such as unsteady RANS equations, DES, SAS, SDES, SBES, or LES are

used to predict the sound with the aid of analytically derived integral solutions to wave equations.

The acoustic analogy essentially decouples the propagation of sound from its generation, allowing

one to separate the flow solution process from the acoustics analysis.

ANSYS Fluent offers a method based on the Ffowcs Williams and Hawkings (FW-H) formulation

[] (p. ). The FW-H formulation adopts the most general form of Lighthill’s acoustic analogy, and

is capable of predicting sound generated by equivalent acoustic sources such as monopoles, dipoles,

and quadrupoles. ANSYS Fluent adopts a time-domain integral formulation wherein time histories of

sound pressure, or acoustic signals, at prescribed receiver locations are directly computed by evaluating

a few surface integrals.

Time-accurate solutions of the flow-field variables, such as pressure, velocity components, and density

on source (emission) surfaces, are required to evaluate the surface integrals. Time-accurate solutions

can be obtained from unsteady Reynolds-averaged Navier-Stokes (URANS) equations, large eddy sim-

ulation (LES), or hybrid RANS-LES models as appropriate for the flow at hand and the features that

you want to capture (for example, vortex shedding). The source surfaces can be placed not only on

impermeable walls, but also on interior (permeable) surfaces, which enables you to account for the

contributions from the quadrupoles enclosed by the source surfaces. Both broadband and tonal noise

can be predicted depending on the nature of the flow (noise source) being considered, turbulence

model employed, and the time scale of the flow resolved in the flow calculation.

The FW-H acoustics model in ANSYS Fluent allows you to select multiple source surfaces and receivers.

It also permits you either to save the source data for a future use, or to carry out an “on the fly”

acoustic calculation simultaneously as the transient flow calculation proceeds, or both. Sound pressure

signals therefore obtained can be processed using the fast Fourier transform (FFT) and associated

postprocessing capabilities to compute and plot such acoustic quantities as the overall sound pressure

level (SPL) and power spectra.

One important limitation of ANSYS Fluent’s FW-H model is that it is applicable only to predicting the

propagation of sound toward free space. Therefore, while the model can be legitimately used to predict

far-field noise due to external aerodynamic flows, such as the flows around ground vehicles and aircraft,

it cannot be used for predicting the noise propagation inside ducts or wall-enclosed space.

In this hybrid simulation method, which is intended to simulate aeroacoustics of low Mach number

flows, the incompressible flow model is used for the calculation of sound sources, while the differential

wave equation is used to calculate the propagation of sound generated by these sources. The acoustics

wave equation implemented in ANSYS Fluent is derived from the acoustics perturbation equations by

Predicting Aerodynamically Generated Noise

Ewert and Schroeder [ref] under the assumption of constant density flow. The main advantages of this

model are:

Extended applicability compared to the Ffowcs Williams and Hawking integral solver, which can be

used only to model the sound propagation in open space (see Integral Method by Ffowcs Williams

and Hawkings (p. )).

Simple and convenient workflow of hybrid aeroacoustics simulations, without any data exchange

between different software components via disk files, and without the interpolation of sound sources

on a different mesh. A transient co-simulation of fluid flow and noise propagation using the same

domain and mesh has been chosen for the current implementation.

In many practical applications involving turbulent flows, noise does not have any distinct tones, and

the sound energy is continuously distributed over a broad range of frequencies. In those situations

involving broadband noise, statistical turbulence quantities readily computable from RANS equations

can be utilized, in conjunction with semi-empirical correlations and Lighthill’s acoustic analogy, to

shed some light on the source of broadband noise.

ANSYS Fluent offers several such source models that enable you to quantify the local contribution (per

unit surface area or volume) to the total acoustic power generated by the flow. They include the fol-

lowing:

Proudman’s formula

jet noise source model

boundary layer noise source model

source terms in the linearized Euler equations

source terms in Lilley’s equation

Considering that one would ultimately want to come up with some measures to mitigate the noise

generated by the flow in question, the source models can be employed to extract useful diagnostics

on the noise source to determine which portion of the flow is primarily responsible for the noise

generation. Note, however, that these source models do not predict the sound at receivers.

Unlike the direct method and the FW-H integral method, the broadband noise source models do not

require transient solutions to any governing fluid dynamics equations. All the source models need is

what typical RANS models would provide, such as the mean velocity field, turbulent kinetic energy ( )

and the dissipation rate ( ). Therefore, the use of broadband noise source models requires the least

computational resources.

The procedure for computing sound using the FW-H acoustics model in ANSYS Fluent consists largely

of two steps. In the first step, a time-accurate flow solution is generated from which time histories of

the relevant variables (for example, pressure, velocity, and density) on the selected source surfaces are

Using the Ffowcs Williams and Hawkings Acoustics Model

obtained. In the second step, sound pressure signals at the user-specified receiver locations are computed

using the source data collected during the first step.

Important

Note that you can also use the FW-H model for a steady-state simulation in the case where

your model has a single moving reference frame. Here, the thickness and loading noise due

to the motion of the noise sources is computed using the FW-H integrals (see Equation .

and Equation . in the Theory Guide), except that the term involving the time derivative

of surface pressure (contribution to

in Equation . in the Theory Guide) is set to zero.

In computing sound pressure using the FW-H integral solution, ANSYS Fluent uses a so-called “forward-

time projection” to account for the time delay between the emission time (the time at which the sound

is emitted from the source) and the reception time (the time at which the sound arrives at the receiver

location). The forward-time projection approach enables you to compute sound at the same time “on

the fly” as the transient flow solution progresses, without having to save the source data.

In this section, the procedure for setting up and using the FW-H acoustics model is outlined first, followed

by detailed descriptions of each of the steps involved. Remember that only the steps that are pertinent

to acoustics modeling are discussed here. For information about the inputs related to other models

that you are using in conjunction with the FW-H acoustics model, see the appropriate sections for those

models.

The general procedure for carrying out an FW-H acoustics calculation in ANSYS Fluent is as follows:

. Calculate a converged flow solution. For a transient case, run the transient solution until you obtain a

“statistically steady-state” solution as described below.

. Enable the FW-H acoustics model and set the associated model parameters.

Setup → Models → Acoustics

Edit...

. Specify the source surface(s) and choose the options associated with acquisition and saving of the source

data. For a steady-state case, specify the rotating surface zone(s) as the source surface(s).

. Specify the receiver location(s).

. Continue the transient solution for a sufficiently long period of time and save the source data (transient

cases only).

Solution →

. Compute and save the sound pressure signals.

Solution →

Run Calculation → Acoustic Signals...

. Postprocess the sound pressure signals.

Solution →

Results → Plots → FFT

Edit...

Important

Before you start the acoustics calculation for a transient case, an ANSYS Fluent transient

solution should have been run to a point where the transient flow field has become “statist-

ically steady”. In practice, this means that the unsteady flow field under consideration, includ-

ing all the major flow variables, has become fully developed in such a way that its statistics

do not change with time. Monitoring the major flow variables at selected points in the domain

is helpful for determining if this condition has been met.

As discussed earlier, URANS, LES, and hybrid RANS-LES models are all legitimate candidates for transient

flow calculations. For stationary source surfaces, the frequency of the aerodynamically generated sound

heard at the receivers is largely determined by the time scale or frequency of the underlying flow.

Therefore, one way to determine the time-step size for the transient computation is to make it small

enough to resolve the smallest characteristic time scale of the flow at hand that can be reproduced by

the mesh and turbulence adopted in your model.

Once you have obtained a statistically stationary flow-field solution, you are ready to acquire the source

data.

... Enabling the FW-H Acoustics Model

... Specifying Source Surfaces

... Specifying Acoustic Receivers

... Specifying the Time Step

... Postprocessing the FW-H Acoustics Model Data

... FFT of Acoustic Sources: Band Analysis and Export of Surface Pressure Spectra

To enable the FW-H acoustics model, select Ffowcs Williams & Hawkings in the Acoustics Model

dialog box (Figure . : The Acoustics Model Dialog Box (p. )).

Edit...

When you select Ffowcs Williams & Hawkings, the dialog box will expand to show the relevant fields

for user inputs.

Figure . : The Acoustics Model Dialog Box

.... Setting Model Constants

Under Model Constants in the Acoustics Model dialog box, specify the relevant acoustic parameters

and constants used by the model.

Far-Field Density

(for example,

in Equation . in the Theory Guide) is the far-field fluid density.

Far-Field Sound Speed

in Equation .) is the sound speed in the far field (=

).

Free Stream Velocity and Free Stream Direction

are required when the convective effects are taken into account.They become available in the interface

when Convective Effects is enabled.

Important

The use of Convective Effects with the proper Free Stream Velocity and Free Stream

Direction is strongly recommended for all cases dealing with external flows around

bodies.

Reference Acoustic Pressure

in Equation . (p. )) is used to calculate the sound pressure level in dB (see Using

the FFT Utility (p. )).The default reference acoustic pressure is

Pa.

Number of Time Steps Per Revolution

is available only for steady-state cases that have a single moving reference frame. Here you will specify

Pa.

the number of equivalent time steps that it will take for the rotating zone to complete one revolution.

Number of Revolutions

the number of revolutions that will be simulated in the model.

Source Correlation Length

is required when sound is to be computed using a 2D flow result.The FW-H integrals will be evaluated

over this length in the depth-wise direction using the identical source data (see Figure . :The Acoustics

Model Dialog Box for a 3D Steady-State Case with a Single Moving Reference Frame (p. )).

The default values are appropriate for sound propagating in air at atmospheric pressure and temper-

ature.

.... Computing Sound “on the Fly”

The FW-H acoustics model in ANSYS Fluent allows you to perform simultaneous calculation of the

sound pressure signals at the prescribed receivers without having to write the source data to files,

which can save a significant amount of disk space on your machine. To enable this “on-the-fly” calcu-

lation of sound, enable the Compute Acoustic Signals Simultaneously option in the Acoustics

Important

Because the noise computation takes a negligible percentage of memory and computa-

tional time compared to a transient flow calculation, this option can be used by itself or

along with the process of source data file export and sound calculation. For the latter,

computing signals “on the fly” allows you to see when the signals have become statistically

steady so you can know when to stop the simulation.

When the Compute Acoustic Signals Simultaneously option is enabled, the ANSYS Fluent console

window will print a message at the end of each time step indicating that the sound pressure signals

have been computed (for example, Computing sound signals at x receiver loca-

tions..., where x is the number of receivers you specified). Enabling this option instructs ANSYS

Fluent to compute sound pressure signals at the end of each time step, which will slightly increase

the computation time.

Important

Note that this option is available only when the FW-H acoustics model has been enabled.

See below for details about exporting source data without enabling the FW-H model.

....Writing Source Data Files

Although the “on-the-fly” capability is a convenient feature, you will want to save the source data as

well, because the acquisition of source data during a transient flow-field calculation is the most time-

consuming part of acoustics computations, and you most likely will not want to discard it. By saving

the source data, you can always reuse it to compute the sound pressure signals at new or additional

receiver locations.

To save the source data to files, enable either the Export Acoustic Source Data in ASD Format or

the Export Acoustic Source Data in CGNS Format option, or both. After you have made your selection,

the relevant source data at all face elements of the selected source surfaces will be written into the

files you specify. The source data vary depending on the solver option you have chosen and whether

the source surface is a wall or not. Table . : Source Data Saved in Source Data Files (p. ) shows

the flow variables saved as the source data.

Figure . : The Acoustics Model Dialog Box for a 3D Steady-State Case with a Single Moving

Reference Frame

Table . : Source Data Saved in Source Data Files

Source Data

Source Surface

Solver Option

walls

permeable surfaces

walls

compressible

See Specifying Source Surfaces (p. ) for details on how to specify parameters for exporting source

data.

..... Exporting Source Data Without Enabling the FW-H Model: Using the ANSYS

Fluent ASD Format

You can export sound source data for use with SYSNOISE without having to enable the Ffowcs Wil-

liams and Hawkings (FW-H) model. You still must specify source surfaces (see Specifying Source

Surfaces (p. )), as .index and .asd files are required by SYSNOISE. In addition, you can choose

fluid zones as emission sources if you want to export quadrupole sources. To enable the selection

of fluid zones as sources, use the

define → models → acoustics → export-volumetric-sources?

text command and change the selection to yes.

SYSNOISE also requires centroid data for source zones that are being exported.

For fan noise calculations, once you have specified the source zones in the Acoustic Sources dialog

box and you have selected Export Acoustic Source Data in ASD Format from the Acoustics

Model dialog box, you can export geometry in cylindrical coordinates by using the

define → models → acoustics → cylindrical-export?

text command and changing the selection to yes. By default, ANSYS Fluent exports source zones

for SYSNOISE in Cartesian coordinates.

You can then export the centroid data to a data file using the following text command:

define → models → acoustics → write-centroid-info

Since you will not be using the FW-H model to compute signals, you will not need to specify any

acoustic model parameters or receiver locations. Also, you will not be able to enable the Compute

Acoustic Signals Simultaneously option in the Acoustics Model dialog box, and Acoustic Signals...

will not be available in the Run Calculation task page and in the menu for the Run Calculation

Outline View item.

..... Exporting Source Data Without Enabling the FW-H Model: Using the CGNS

Format

The sound source data for non-permeable surfaces can be exported in the CGNS file format (for

Virtual Lab) without having to enable the Ffowcs Williams and Hawkings (FW-H) model. Enable the

Export Acoustic Source Data in CGNS Format option in the Acoustics Model dialog box (Fig-

ure . : The Acoustics Model Dialog Box for Exporting in CGNS Format (p. )). Specify the source

surfaces in the Acoustics Sources dialog box (see Specifying Source Surfaces (p. )) where, by

default, the Number of Time Steps per File is set to .

Note

The following limitations currently exist for exporting acoustic source data:

ANSYS Fluent does not support exporting acoustic source data in CGNS format for polyhedral

meshes.

Source data cannot be simultaneously exported for multiple differently rotating walls. All

walls must be either non-rotating, or rotate with the same rate around the same axis.

meshes.

Figure . : The Acoustics Model Dialog Box for Exporting in CGNS Format

Virtual Lab requires a mesh data file (named <prefix>_mesh.cgns) and a solution data file

(named <prefix>_<timestep>.cgns). The string <prefix> is a generic name, which you will

specify in the File Name in the Acoustics Sources dialog box. There is one single solution data file

(.cgns) per time level exported, which contains the static pressure at the wall-face centroid location.

The .cgns files will be stored in a directory, which you specify (named <directory_name>/<pre-

fix>) in the File Name.

In addition, you can export quadrupole sources data by choosing fluid zones as emission sources.

To enable the selection of fluid zones as sources, use the text command:

define → models → acoustics → export-volumetric-sources-cgns?

When asked if you would like to Export volumetric sources? enter yes. Note that Virtual

Lab requires volumetric mesh data file (<prefix>_Q_mesh.cgns) and quadrupole solution data

files (<prefix>_Q_<timestep>.cgns). The .cgns file will be stored in a similar way to that of

dipole data export, in the directory you specified in the File Name text entry box.

In the Acoustics Model dialog box, click the Define Sources... button to open the Acoustic Sources

dialog box (Figure . : The Acoustics Model Dialog Box (p. )). Here you will specify the source sur-

face(s) to be used in the acoustics calculation and the inputs associated with saving source data to

files.

files.

Under Source Zones, you can select multiple emission (source) surfaces and the surface Type that

you can select is not limited to a wall. You can also choose interior surfaces and sliding interfaces

(both stationary and rotating) as source surfaces.

Important

The ability to choose multiple source surfaces is useful for investigating the contributions

from individual source surfaces. The results based on the use of multiple source surfaces

are valid as long as there are negligible acoustic interactions among the surfaces. Therefore,

some caution should be taken when selecting multiple source surfaces.

In cases where multiple source surfaces are selected, no source surface may enclose any of the other

source surfaces. Otherwise, the sound pressure calculated based on the source surfaces will not be

accurate, as the contribution from the enclosed (inner) source surfaces is over predicted, since the FW-

H model is unable to account for the shading of the sound from the inner source surfaces by the en-

closure surface.

If you specify any interior surfaces as source surfaces, the interior surface must be generated in advance

(for example, in GAMBIT) in such a way that the two cell zones adjacent to the surface have different

cell zone IDs. Furthermore, you must correctly specify which of the two zones is occupied by the

quadrupole sources (interior cell zone). This will allow ANSYS Fluent to determine the direction in

which the sound will propagate. When you first attempt to select a legitimate interior surface (that is,

an interior surface having two different cell zones on both sides) as a source surface, the Interior Cell

Zone Selection Dialog Box (p. ) (Figure . : The Interior Cell Zone Selection Dialog Box (p. )) will

appear. You must then select the interior cell zones from the two zones listed under the Interior Cell

Zone. Figure . : An Interior Source Surface (p. ) shows an example of an interior source surface.

Figure . : The Interior Cell Zone Selection Dialog Box

Like general interior surfaces, if the source surfaces selected are sliding interfaces, a dialog box similar

to Figure . : The Interior Cell Zone Selection Dialog Box (p. ) will appear that will show the two

adjacent cell zones and you will be asked to specify the zone that has the sound sources.

Important

When a permeable surface (either interior or sliding interface) is chosen as the source surface,

other wall surfaces inside the volume enclosed by the permeable surface that generate

sound should not be chosen for the acoustics calculation. For example, when running an

“on-the-fly” calculation, if both these surfaces are selected, the sound pressure will be

counted twice.

Figure . : An Interior Source Surface

.... Saving Source Data

To save the source data, you have to specify the File Name, Write Frequency (in number of time

steps), and Number of Time Steps per File in the Acoustic Sources dialog box.

The File Name is used to give the names of the source data files (for example, acoustic_ex-

amplexxxx.asd, where xxxx is the global time-step index of the transient solution) and an index

file (for example, acoustic_example.index) that will store the information associated with the

source data. The Write Frequency allows you to control how often the source data will be written.

This will enable you to save disk space if the time-step size used in the transient flow simulation is

smaller than necessary to resolve the sound frequency you are attempting to predict. In most situations,

however, you will want to save the source data at every time step and use the default value of .

Since acoustics calculations usually generate thousands of time steps of source data, you may want

to split the data into several files. Specifying the Number of Time Steps per File allows you to write

the source data into separate files for different simulation intervals, the duration of which (in terms

of the number of transient flow time steps) is specified by you. For example, if you specify  for

this parameter, each file will contain source data for an interval length of  time steps regardless

of the write frequency.

You will find this feature useful if you want to use a selected number of source data files to compute

the sound pressure rather than using all the data. For example, you may want to exclude an initial

portion of the source data from your acoustics calculation because you may realize later that the flow

field has not fully attained a statistically steady state.

After you click Apply, ANSYS Fluent will create the index file (for example, acoustics_example.in-

dex), which contains information about the source data.

Important

Important

If you choose to save source data, keep in mind that the source data can use up a consid-

erable amount of disk space, especially if the mesh being used has a large number of face

elements on the source surfaces you selected. ANSYS Fluent will print out the disk space

requirement per time step at the time of source surface selection if the Export Acoustic

Source Data in ASD Format option is enabled in the Acoustics Model dialog box.

At this point, if you have chosen to perform your acoustics calculation in two steps, (that is, saving

the source data first, and computing the sound at a later time), you can go ahead and instruct ANSYS

Fluent to perform a suitable number of time steps, and the source data will be saved to the disk. If

you chose to perform an “on-the-fly” acoustic calculation, then you must specify receiver locations

(see Specifying Acoustic Receivers (p. )) before you run the unsteady ANSYS Fluent solution any

further.

In the Acoustics Model dialog box, click the Define Receivers... button to open the Acoustic Receivers

dialog box (Figure . : The Acoustic Receivers Dialog Box (p. )).

Figure . : The Acoustic Receivers Dialog Box

Important

Note that you can also open the Acoustic Receivers dialog box by clicking the Receivers...

button in the Acoustic Sources or the Acoustic Signals dialog box.

If required, you can enable Moving Receivers to specify the receiver motion. In this case, the defined

Velocity magnitude and Direction apply to all receivers. The receiver locations, defined below, are

then interpreted as the starting locations at the time that sound emission originates. The origination

of sound emission is determined as follows:

For “on the Fly” use of the FW-H model (see Computing Sound “on the Fly” (p. )) the sound emission

time is counted from the physical time of activation of the Compute Acoustic Signals Simultaneously

option (see Figure . :The Acoustics Model Dialog Box (p. )).

When the FW-H model reads the previously written acoustic source data (see Reading Unsteady

Acoustic Source Data (p. )), the sound emission time starts from the physical time associated with

the first selected source data file.

Important

When using moving receivers, note that if you start from a different source data file,

this results in different receiver locations due to the different emission time origin as-

sociated with the different source data file.

Increase the Number of Receivers to the total number of receivers for which you want to compute

sound, and enter the coordinates for each receiver in the X-Coord., Y-Coord., and Z-Coord. fields.

Note that because ANSYS Fluent’s acoustics model is ideally suited for far-field noise prediction, the

receiver locations you define should be at a reasonable distance from the sources of sound (that is,

the selected source surfaces). The receiver locations can also fall outside of the computational domain.

For each receiver, you can specify a file name in the Signal File Name field. These files will be used

to store the sound pressure signals at the corresponding receivers. By default, the files will be named

receiver-.ard, receiver-.ard, and so on.

Once the receiver locations have been defined, the setup for your acoustic calculation is complete.

When using an implicit-in-time solution algorithm (dual-time stepping), and depending on the physical

time step size and the most important time scales in the flow, you can write the acoustic source data

at every time step. You can also coarsen it in time by a given frequency factor. The highest possible

frequency the acoustic analysis can generate is based on the time step size of the collected acoustic

source data.

When using the Density-Based explicit solver, with the Explicit Transient Formulation selected in

the Solution Methods task page, the physical time step must be computed by the solver, based on

the CFL condition (Courant number). Due to the possibly large fluctuations of the physical time step,

an adapting time-stepping procedure can be used when the FW-H acoustics model is enabled. This

allows you to use a user-specified time interval for sampling the acoustic data. In turn, the solver adapts

its time step, when necessary, without violating the CFL conditions to make sure that data is available

at the desired time interval (hence, avoiding data interpolations).

In the Run Calculation task page (Figure . : The Run Calculation Task Page (p. )), enter the Time

Step Size for Acoustic Data Export to specify the time interval for acoustic data sampling. The value

of this constant time step size determines the highest frequency that the acoustic analysis reproduces.

You can refer to Performing Time-Dependent Calculations (p. ) for more information about the Run

Solution →

Figure . : The Run Calculation Task Page

You can now proceed to instruct ANSYS Fluent to perform a transient calculation for a suitable number

of time steps. When the calculation is finished, you will have either the source data saved on files (if

you chose to save it to a file or files), or the sound pressure signals (if you chose to perform an

acoustic calculation “on the fly”), or both (if you chose to save the source data to files and if you chose

to perform the acoustic calculation “on the fly”).

If you chose to save the source data to files, the ANSYS Fluent console will print a message at the end

of each time step indicating that source data have been written (or appended to) a file (for example,

acoustic_example240.asd).

At this point, you will have either the source data saved to files or the sound pressure signals computed,

or both. You can process these data to compute and plot various acoustic quantities using ANSYS

Fluent’s FFT capabilities. See Fast Fourier Transform (FFT) Postprocessing (p. ) for more information.

....Writing Acoustic Signals

If you chose to perform the acoustic calculation “on the fly”, you must write the sound pressure data

to files. To do so, select Write Acoustic Signals under Options in the Acoustic Signals dialog box

(Figure . : The Acoustic Signals Dialog Box (p. )) and then click Write. The computed acoustic

pressure will be saved from internal buffer memory into a separate file for each receiver you defined

in the Acoustic Receivers dialog box (for example, receiver-.ard).

Solution →

.... Reading Unsteady Acoustic Source Data

Computing the sound pressure signals using the source data saved to files is done in the Acoustic

Signals dialog box (Figure . : The Acoustic Signals Dialog Box (p. ))

Solution →

Figure . : The Acoustic Signals Dialog Box

To compute the sound data, use the following procedure:

. In the Acoustic Signals dialog box, select Read Unsteady Acoustic Source Data Files under Options.

. Click Load Index File... and select the index file for your computation in the Select File dialog box.The

file will have the name you entered in the File Name field in the Acoustic Sources dialog box, followed

by the .index suffix (for example, acoustic_example.index).

. In the Source Data Files list, select the source data files that you want to use to compute sound. Source

data files will all contain the specified root file name followed by the suffix .asd.

Important

You can use any number of source data files. However, note that you should select

only consecutive files.

Important

. In the Active Source Zones list, select the source zones you want to include to compute sound. See

Specifying Source Surfaces (p. ) for details about proper source surface selection.

. In the Receivers list, select the receivers for which you want to compute and save sound.

Optionally, you can click the Receivers... button to open the Acoustic Receivers dialog box and

define additional receivers.

. Click the Compute/Write button to compute and save the sound pressure data. One file will be saved

for each receiver you previously specified in the Acoustic Receivers dialog box (for example, receiver-

.ard).

Important

If you enabled both the Export Acoustic Source Data in ASD Format and Compute

Acoustic Signals Simultaneously options in the Acoustics Model dialog box, you must

first select the Write Acoustic Signals option in the Acoustic Signals dialog box after the

flow simulation has been completed. If you select the Read Unsteady Acoustic Source

Data Files before writing out the “on-the-fly” data in such a case, the data will be flushed

out of the internal buffer memory. To avoid such a loss of data, you should save the ANSYS

Fluent case and data files whenever you begin to do an acoustic computation in the

Acoustic Signals dialog box. The sound pressure data calculated “on the fly” will then be

saved into the .dat file. Finally, after the “on-the-fly” data is saved, make sure to change

the file names of the receivers before doing a sound pressure calculation with the Read

Unsteady Acoustic Source Data Files option enabled, to avoid overwriting the “on-the-

fly” signal files.

Important

Important

Note that you can compute and write sound pressure signals only when the FW-H acoustics

model has been enabled. See Exporting Source Data Without Enabling the FW-H Model:

Using the ANSYS Fluent ASD Format (p. ) for details about exporting source data (for

example, for SYSNOISE) without enabling the FW-H model.

..... Pruning the Signal Data Automatically

Before the computed sound pressure data at each receiver is saved, it is by default automatically

pruned. Pruning of the receiver data means clipping the tails of the signal where incomplete source

information is available.

The acoustic source data is tabulated from time

to

. Without auto-pruning, the receiver register

begins receiving the earliest sound pressure signal at

(.)

where

is the shortest distance between the source surfaces and the receiver. However, the re-

ceiver will not receive the sound pressure signal from the farthest point on the source surfaces (

)

until the receiver time becomes

(.)

From time  to , the sound accumulated on the receiver register does not include the contribution

from the entire source surface area, and therefore the sound pressure data received during that time

is not complete. The same thing occurs during the period from

(.)

to

(.)

Therefore, pruning means clipping the signal on the incomplete ends, from  to  and

to

.

Auto-pruning can be disabled using the define → models → acoustics → auto-prune text

command. Although auto-pruning can be disabled, it is expected that you will use only the complete

sound pressure data.

.... Reporting the Static Pressure Time Derivative

The RMS value of the static pressure time derivative (

) is available for postprocessing only on

wall surfaces, which are at the same time sources of sound, when the FW-H acoustics model is used.

You can select Surface dpdt RMS in the Acoustics... category only when you specify at least one

wall surface, which is also marked as an acoustic source, in the relevant postprocessing dialog boxes.

.... Using the FFT Capabilities for Sound Pressure Signals

Once the sound pressure signals are computed and saved in files, the sound data is ready to be

analyzed using ANSYS Fluent’s FFT tools. In the Fourier Transform dialog box (Figure . : The

Fourier Transform Dialog Box (p. )), click Load Input File... and select the appropriate .ard file.

If the receiver data is still in ANSYS Fluent’s memory, then it can directly be processed using the

Process Receiver option. See Fast Fourier Transform (FFT) Postprocessing (p. ) for more information

on ANSYS Fluent’s FFT capabilities.

Edit...

... FFT of Acoustic Sources: Band Analysis and Export of Surface Pressure

Spectra

During a transient flow simulation, the time histories of the instant surface pressure values can be

written into the binary acoustic source data (ASD) files. This operation is performed for all mesh cell

faces of those surface zones that are selected as acoustic sources. The primary purpose of the ASD

files is to supply input data for the Ffowcs Williams and Hawkings acoustic solver (see Reading Unsteady

Acoustic Source Data (p. )). Additionally, these files can be used to visualize the spectral properties

of the stored flow pressure signals. The supported spectral properties are the complex amplitudes for

the individual Fourier modes, and the surface pressure level (SPL) values for the frequency bands, in

decibels. Both the constant width and the proportional width bands (octaves and / octaves) can be

Note

Despite the use of the common acronym “SPL”, the calculated values characterize the

transient flow pressure on a surface, and not the acoustic pressure; that is, in this context,

the acronym refers to the “Surface Pressure Level” (as mentioned previously) and not the

“Sound Pressure Level”.

In addition to the visualization capabilities, with ANSYS Fluent you can also use the ASD files to export

the computed spectrum fields of the flow pressure as CGNS files. The primary purpose of such files is

to allow you to use the surface spectrum fields as distributed excitation forces when performing a

harmonic response analysis with ANSYS Mechanical. The ability to import CGNS files is available in

ANSYS Mechanical to match this export feature in Fluent; for details, see FLUREAD in the separate

Mechanical APDL Command Reference. Using the acoustic wave equation solver of ANSYS Mechanical,

it is possible to perform frequency domain simulations for applications such as the vehicle cabin noise

caused by external turbulent flow.

.... Using the FFT of Acoustic Sources

The Acoustic Sources FFT… button is available in the Run Calculation task page under the following

conditions:

The simulation is set up as a three-dimensional transient case.

The Export Acoustic Source Data in ASD Format option is enabled in the Acoustics Model dialog box.

Clicking the Acoustic Sources FFT… button opens the Acoustic Sources FFT dialog box, which has

four tabs (each of which is shown in the figures that follow):

Read ASD Files

Compute FFT Fields

FFT Surface Variables

Write CGNS Files

The first two tabs are obligatory, because the actions performed there prepare the Fourier spectra

for the actions that follow, including creation of the surface variables to visualize (performed in the

third tab) and/or CGNS export (performed in the fourth tab).

Postprocessing begins in the Read ASD Files tab. The Active Source Zones selection list shows all

of the face zones for which transient export to ASD files has been performed (see Figure . : The

Read ASD Files Tab of the Acoustic Source FFT Dialog Box (p. )). The Source Data Files selection

list shows all of the available ASD files. Note that you can update this information by clicking the

Load Index File… button and specifying the name of the index file to be read; the index file was

created during the ASD files export, and is an ASCII file containing a list of the source zones and a

list of the ASD file names. Select in the selection lists the desired face zones as well as the desired

ASD files from which you want to read, and click the Read button. The console displays information

about the data, such as the following example:

Overall  timesteps have been read

from . s to  s

Time step is . s

from . s to  s

Figure . : The Read ASD Files Tab of the Acoustic Source FFT Dialog Box

Having read the pressure histories, open the Compute FFT Fields tab (Figure . : The Compute

FFT Fields Tab of the Acoustic Source FFT Dialog Box (p. )). The values shown in the Spectral

Resolution group box provide information about the statistical properties, which depend on the

sampling rate (that is, the simulation time step) and the signal length (that is, the simulation time).

These values will change if you enable the Clip Time to Range option in the Sampling Data group

box, reduce the time range for the signals by changing the Min and/or Max fields, and click the Re-

Estimate Spectral Resolution button. The Window Function selection list allows you to specify a

window function using the same choices that are available for plotting the single signal FFT in the

Plot/Modify Input Signal dialog box. The default settings use the full signals and the Hanning window

function. The FFT calculation begins when you click the Compute button.

Figure . : The Compute FFT Fields Tab of the Acoustic Source FFT Dialog Box

The fields of the pressure histories and the computed fields of the Fourier spectra are stored in a

large memory array, referred to here as the “storage area”. This memory is allocated by Fluent dynam-

ically when you read the pressure signals from the ASD files. If you read data for all face zones available

in the ASD files, and if they are the wall zones, then the size of the allocated storage area is equal to

the total size of the ASD files being read. Since the same or a slightly smaller amount of data is pro-

duced by the FFT algorithm, the same storage area can be re-used to store the Fourier spectra without

allocating additional memory. Alternatively, the pressure histories can be left intact in memory, and

for their spectra the storage area is correspondingly increased.

These two modes of memory allocation are controlled by the Overwrite Signals by Spectra option

in the Storage Area Control group box. When the Overwrite Signals by Spectra option is enabled,

the Fourier spectra displace in memory the original time signals, which are not kept after the FFT has

been computed. Therefore, if you want to re-compute the FFT using the Clip Time to Range tool or

a different Window Function (which are both in the Compute FFT Fields tab), you have to first de-

allocate the storage area by clicking the Clean Up Entire Storage Area button, and then re-read the

pressure histories from the ASD files. When the Overwrite Signals by Spectra option is disabled,

you can re-compute the FFT without re-reading the pressure histories, as many times as you want.

To do this, click the Clean Up Only FFT Results button, and proceed with computing spectra from

the available pressure histories. De-allocation of the storage area (which can be very large) is recom-

mended when you are done using the Acoustic Sources FFT dialog box and plan to either proceed

to other postprocessing work or continue your transient simulation without re-starting Fluent.

When the pressure histories are read and kept in the storage area, you can create point probes

within the surface zones that have been read and extract the single pressure time signals at these

probes. The extracted signals and their spectra may help to analyze the transient flow properties. For

example, by creating an XY plot of a signal, you can figure out the need for clipping of the sampling

time; by creating an XY plot of its spectrum, you can detect the presence of the tonal noise compon-

ents.

To create a point probe, open the Point Surface Dialog Box (p. ) by clicking Create and selecting

Point... in the Domain ribbon tab (Surface group box), and create a point surface by any available

method (for example, by specifying the coordinates). The point probe will be created at the face

center that is nearest to the point surface on the read surface zones. The created point probes are

then listed under the point surface names in the Existing Points selection list, which is located in

the Point Probes for Time Signals group box. You can print the coordinates of the point probes to

the Fluent console by selecting the desired probes and clicking the Print Coordinates button. Clicking

the Extract Signals button outputs the pressure histories for the selected probes in the ASCII files;

these files can then be analyzed using the Fourier Transform Dialog Box (p. ) (available from the

Plots Task Page (p. )) by selecting Process File Data and then reading the exported ASCII file using

the Load Input File... button. The exported files names are by default the point probe names with

the extension .dat. The File Name field allows you to specify a prefix for these file names.

The FFT Surface Variables tab is shown in Figure . : The FFT Surface Variables Tab of the Acoustic

Source FFT Dialog Box for the Octave Bands (p. ) and Figure . : The FFT Surface Variables Tab

of the Acoustic Source FFT Dialog Box for a Set of Individual Modes (p. ). This tab allows you to

Create new Fluent variables using the computed spectrum fields, which reside in the storage area

and correspondingly increase its size. These variables will be defined only on those wall face zones

for which the Fourier transformation has been computed; on the other face zones, they will show

zero values. Created variables can be used for any kind of further postprocessing in Fluent, which

typically includes contour plotting (see the variables marked with the restriction asfft in Table . :

Acoustics Category (p. )) or exporting to CFD-Post.

Figure . : The FFT Surface Variables Tab of the Acoustic Source FFT Dialog Box for the Octave

Bands

Variables may characterize either the individual Fourier modes (if you select Set of Modes from the

Modes/Frequency Bands drop-down list), or frequency bands that each represent a range of frequen-

cies (if you select the other choices in the Modes/Frequency Bands drop-down list). The three types

of frequency bands that are available include:

Octave Bands

These are proportional bands corresponding to the standard technical octaves.

/ Octave Bands

These are proportional bands corresponding to the standard technical thirds.

Constant Width Bands

These are user-defined equidistant bands.

The Spectrum Property drop-down list displays the type of variables created according to the selected

choice in the Modes/Frequency Bands drop-down list. For a set of modes, the created variables are

the real and the imaginary parts of the complex Fourier amplitudes, with a pair of variables per specified

mode. For the frequency bands, the created variables are the surface pressure level (SPL) fields, in

decibels. The transformation to the decibel units is done by default using the standard acoustic refer-

ence pressure value of  x - Pa; you can change this value before creating the variables by opening

the Acoustic Models dialog box, selecting the Ffowcs Williams & Hawkings model, and revising

the Reference Acoustic Pressure.

For any type of frequency band (octave, /, or constant width), the area-averaged band-specific

pressure fluctuations are calculated and printed out to the Fluent console in decibels when you click

Create. Conversion to decibels is done after the area-averaging of the band-filtered RMS pressure

fluctuation fields. The area-averaged data is printed only for those frequency bands that are covered

by the resulting pressure spectrum. If you enable the Write Area-Avg Data option and specify a file

name in the corresponding field, then the area-averaged data will be written to an ASCII file in the

XY plot file format (see XY Plot File Format (p. )). It is recommended that you use the file name

extension .xy to more easily recognize this file when using the XY plotting tool.

If you enable the Plot Area-Avg Data option, then the data will be plotted in the form of a bar chart

in the graphics window when you click Create, as shown in Figure . : Bar Chart of Surface Pressure

Level for Octave Bands (p. ).

Figure . : Bar Chart of Surface Pressure Level for Octave Bands

Figure . : The FFT Surface Variables Tab of the Acoustic Source FFT Dialog Box for a Set of

Individual Modes

The allowed number of variables makes it possible for you to simultaneously keep SPL for all octave

and / octave bands, as well as SPL for up to  constant width bands and the real and imaginary

amplitudes for up to  individual frequencies. The SPL variables for the octaves and the / octaves

include the band central frequency in their names (for example, SPL for Octave Band at 250Hz (dB)

or SPL for /-Octave Band at .25kHz (dB)). As for the user-defined frequencies and constant width

bands, their variables are simply numbered from  to . In order to provide you with the information

about the meaning of each such variable, Fluent prints a table in the console when you click Create.

The following is an example of the table corresponding to the settings in the previous figure:

Creating variables for  modes from . Hz to . Hz every . Hz.

f( ) = . Hz     f( ) = . Hz

f() = . Hz     f() = . Hz

Variables for frequencies above . Hz are not created,

because the limit of  modes has been reached.

You can analyze more than  individual modes or constant width bands, if you process them by

portions of  items and delete the processed variables by selecting them in the Existing Variables

list and clicking the Remove Selected Variables button.

Clicking either the Clean Up Entire Storage Area or the Clean Up Only FFT Results button on the

left side of the dialog box not only de-allocates the spectrum storage array, but also removes all

created variables.

The Write CGNS Files tab is shown in Figure . : The Write CGNS Files Tab of the Acoustic Source

FFT Dialog Box (p. ). This tab allows you to specify the zones you want to export to CGNS, by se-

lecting them in the Processed Source Zones list. You can reduce the exported spectrum data by

enabling the Reduce Frequency Series option and specifying the frequency range (Min and Max

frequencies), as well as the frequency step (the Number of Frequencies to Skip integer field). The

latter must be used with care and only if really needed, because the Fourier amplitudes in the

broadband noise spectrum depend on the frequency resolution. By skipping frequencies from the

exported spectrum (for example, exporting every other Fourier mode), you will artificially coarsen the

frequency resolution. However, the exported amplitudes will not be automatically re-scaled for the

increased frequency step, but will retain their originally computed values.

Pressure spectra, which result from the scale-resolving flow simulations, may contain thousands of

frequencies. Together with dense surface meshes, this can result in a very large amount of data to

export. The total size of the disk space required to store fields of the complete spectra is approximately

equal to the total size of the ASD files containing the wall pressure histories. Therefore, the wall

pressure spectra are written to a series of CGNS files according to the Number of Frequencies per

File field. It is recommended that you select an appropriate value for this parameter, to avoid extremely

large output files or a large number of very small files. The total number of frequencies in the spectrum

can be seen in the Number of Modes field of the Compute FFT Fields tab (see Figure . : The

Compute FFT Fields Tab of the Acoustic Source FFT Dialog Box (p. )).

Figure . : The Write CGNS Files Tab of the Acoustic Source FFT Dialog Box

Finally, you can specify a name for the exported CGNS files in the File Name field. For example, if

you enter wall_pressure_spectrum and then click the Write button, Fluent will create the fol-

lowing set of files in your working folder:

wall_pressure_spectrum.cgns

wall_pressure_spectrum_1.cgns

wall_pressure_spectrum_2.cgns

...

wall_pressure_spectrum.flst

If you leave the File Name field empty, the files will be named cgns, .cgns, .cgns, ..., flst. The first

CGNS file (without a number in its name) contains the mesh data, as well as links to all of the other

CGNS files, which in turn contain the spectrum fields with the specified number of modes per file.

The CGNS links work like the file links in the UNIX file system: in order to import spectra to the ANSYS

Mechanical software, you only have to specify the name of the first file, and all other files will be im-

ported automatically if they reside in the same folder. The file with the extension flst is an ASCII file,

which contains the list of the exported frequencies.

Important

You should not specify a relative path as a part of the File Name input. If you do that, all files

will be exported in the desired folder according to the specified path. However, the CGNS links,

which are written in the first CGNS file, will also include the specified path.Therefore, the linked

CGNS files will become readable only after the correspondent file relocation—for example,

moving the first CGNS file in your Fluent working folder.

The public domain CGNS library, which is used to process CGNS files in Fluent and ANSYS

Mechanical, has a performance issue when run on Windows. Namely, for CGNS files that have

many links (as is the case in this application), the input / output operations may be very slow

if the CGNS files are located on a network disk.Therefore, for Windows it is strongly recommen-

ded that you select either a built-in local disk or a USB disk directly connected to your computer

as the location of the CGNS files.This warning concerns both the export of CGNS files from

Fluent and their import in ANSYS Mechanical.

The acoustics wave equation model is recommended to be used with scale-resolving simulations of

turbulent flows at low Mach numbers (LES, SBES, DES, SAS). Due to the current limitation of constant

density and sound speed in the background fluid flow, no significant variation of these two parameters

due to non-uniform temperature or mixture composition is allowed.

It is highly recommended that you read Preventing Non-Physical Reflections of Sound Waves in the

Fluent Theory Guide for strategies to improve simulation quality.

The wave equation model is available for transient flow simulations with the second order or bounded

second order implicit time scheme active. The model is not available for the -D axisymmetric version

of Fluent.

You can enable the Wave Equation using the TUI command:

/define/models/acoustics/wave-equation?

The wave equation options are found in the menu:

/define/models/acoustics/wave-equation-options

The field Artificial Viscosity Factor for Sponge Layer is used to specify parameter C, which participates

in Equation .. The base level of artificial viscosity  can be changed by the TUI command:

/define/models/acoustics/wave-equation-options/sponge-layer-base-level

The far-field parameters can be set using the TUI command:

/define/models/acoustics/far-field-parameters

... Specifying Source Mask and Sponge Regions

The Acoustics Region group box is used to set up the geometry of the source mask and sponge regions.

Using the Acoustics Wave Equation Model

There are two methods to define geometry data:

Preparing UDFs

Use of basic shapes (rectangular hexahedron, cylinder, sphere)

The two methods may be combined together. The source mask and the sponge layer UDFs are created

using the following macros:

DEFINE_SOURCE_MASK(src_mask_define, c, t)

DEFINE_SPONGE_LAYER(sponge_define, c, t)

where src_mask_define and sponge_define are example function names, c is a cell number,

and t is a pointer to a cell thread. There can only be one UDF of each of these two types per simulation.

Each UDF returns a single real value, which fills a corresponding storage variable (SV_SOUND_MOD-

EL_SRC_MASK or SV_SOUND_SPONGE) in the cell c of the thread t.

Simple geometries can be built out of the basic shapes (rectangular hexahedron, cylinder, sphere),

which must be preliminarily defined as cell registers of the type Region.

Important

The cell registers must be created using the Outline View path (

Solution → Cell Re-

gisters

New → Region..) and not the ribbon path (

→ Domain → Adapt →

Mark/Adapt Cells → Region..., which is only available if you have used the following text

command: mesh/adapt/revert-to-R19.-user-interface).

The latter path creates older style registers that cannot be used for source mask and sponge

geometry definitions. The appropriate TUI commands to create and edit cell registers are

located in the menu /solve/cell-registers.

After you create one or more cell registers, you can use them to specify the desired geometry by

clicking Basic Shapes... in the Acoustics Model dialog box (Figure . : The Acoustics Model Dialog

Box (p. )), which opens the Basic Shapes dialog box (Figure . : The Basic Shapes Dialog

Box (p. )). In this window you can add cell registers to either the source mask or sponge layer geo-

metry definitions, and specify the individual transition thickness for each shape for each purpose.

Note

After the cell registers have been used for the source mask and sponge layer geometry

definitions, subsequent editing or deleting of these cell registers do not influence the already

specified source mask and sponge layer geometry.

Figure . : The Basic Shapes Dialog Box

The TUI commands for creating and editing source mask and sponge later geometry can be found in

the menu:

/define/models/acoustics/wave-equation-options/basic-shapes/

To visualize the source mask and the sponge layer geometries, use the field variables Sound WaveEq

Model Source Mask and Sound Sponge Layer Marker from the Acoustics… variable group.

These output fields directly show the storage variables SV_SOUND_MODEL_SRC_MASK and

SV_SOUND_SPONGE without any transformations.

... Solution Controls for the Acoustics Wave Equation

When the wave equation model is active, the Solution Controls task page includes an additional

frame titled Acoustics Wave Equation Solver Controls (see Figure . : The Acoustics Wave Equation

Solver Controls Task Page (p. )).

Figure . : The Acoustics Wave Equation Solver Controls Task Page

The parameters Relative Convergence Criterion and Max Iterations/Time Step control the sub-iter-

ations of the implicit wave equation solver. The need for sub-iterations comes from explicit skewness

corrections to the discretization of the basic Laplacian term in Equation ., as well as the artificial

viscosity term. At each sub-iteration, the system of linear equations is processed by the AMG linear

solver to reduce the residual norm by a factor of . (this can be controlled by changing the rp-variable

acoustics-waveeq/amg-alpha). The optimal values of these three algorithm parameters may

depend on the mesh quality. Their default values may change in future releases after accumulating

more experience with the wave equation model.

The TUI commands for the acoustics wave equation solution controls are found in the menu:

/solve/set/acoustics-wave-equation-controls/

The sub-menu /expert allows you to specify under-relaxation factors to enforce convergence on

low quality meshes. Under normal circumstances, under-relaxation is not recommended.

... Solution Initialization

The wave equation model is to be activated after the development of a time-dependent flow solution.

Therefore the acoustics field requires a separate initialization process, that includes ramping in time

the sound source term found in Equation .. With the wave equation model enabled, a Sound

Potential field and a new button Initialize Acoustics… appear on the Solution Initialization task

page. The initial Sound Potential value should always be kept at zero. The Initialize Acoustics…

button opens the Acoustics Initialization dialog box (Figure . : The Acoustics Initialization Dialog

Box (p. )), where you can specify the number of timesteps for the ramping process.

Figure . : The Acoustics Initialization Dialog Box

You can re-initialize the acoustics field separately at any time, since it does not influence the transient

flow solution which is simply continued further.

You can specify the number of timesteps for the ramping process using the TUI command:

/solve/initialize/init-acoustics-options

Note

If you enable the wave equation model in a non-initialized setup, then the initialization of

the entire simulation will also initialize acoustics. However the ramping duration will be set

to zero. You can reset the ramping process by re-initializing acoustics separately.

... Post-Processing

The following field variables are available in the Acoustics… group for post-processing:

– main practical interest, connected to the sound potential by Equation .. The sound pressure

field is less smooth than the sound potential field because of numerical differentiation.

– primary solution variable.

Sound DP/Dt

– time derivative of the sound pressure (a second time derivative of the primary solution variable).

This field may display a lot of noise.

– original model source term.

Sound WaveEq Model Source Smoothed

– source term smoothed by the time filter.

– source masking marker.

– sponge layer marker.

Note

Both the Sound WaveEq Model Source and Sound WaveEq Model Source Smoothed do

not include the effects of source masking and ramping. In order to see the source field after

the application of masking and ramping, you can use the expert output field Sound WaveEq

Source in the Acoustics… group, which can be enabled by responding “yes” to the question

Keep temporary solver memory from being freed?

in the TUI command dialog of /solve/set/expert.

In this section, the procedure for setting up and using the broadband noise source models is outlined

first, followed by descriptions of each of the steps involved.

The general procedure for carrying out a broadband noise source calculation in ANSYS Fluent is as follows:

. Calculate a steady or unsteady RANS solution.

. Enable the broadband noise model and set the associated model parameters.

Edit...

. Postprocess the noise sources.

Edit...

... Enabling the Broadband Noise Source Models

... Postprocessing the Broadband Noise Source Model Data

To enable the broadband noise sources models, select Broadband Noise Sources in the Acoustics

Model dialog box (Figure . : The Acoustics Model Dialog Box for Broadband Noise (p. )).

Edit...

Figure . : The Acoustics Model Dialog Box for Broadband Noise

and constants used by the model. See Enabling the FW-H Acoustics Model (p. ) for the definitions

of Far-Field Density and Far-Field Sound Speed.

Using the Broadband Noise Source Models

Reference Acoustic Power

in Equation . in the Theory Guide) is used to compute the acoustic power outputs

in decibels (dB).The default value is

. Note that the units for the reference acoustic power will be

different in 2D (W/m2) and 3D (W/m3) cases.

Number of Realizations

is the number of samples used in the SNGR to compute the averaged source terms of LEE and Lilley’s

equations.The default value is .

Number of Fourier Modes

(

in Equation . in the Theory Guide) is the number of the Fourier modes used to compute the

turbulent velocity field and its derivatives.The turbulent velocity field is then used to compute the LEE

and Lilley’s source terms.The default value is .

The final step in the broadband noise source modeling process is the postprocessing of acoustic power

and noise source data. The following variables are available in the Acoustics... postprocessing category:

Jet Acoustic Power Level (dB) (axisymmetric models only)

Jet Acoustic Power (axisymmetric models only)

Lilley’s Self-Noise Source

Lilley’s Shear-Noise Source

Lilley’s Total Noise Source

LEE Self-Noise Z-Source (3D models only)

LEE Shear-Noise Z-Source (3D models only)

LEE Total Noise Z-Source (3D models only)

Chapter : Modeling Discrete Phase

This chapter describes how to use the Lagrangian discrete phase capabilities available in ANSYS Fluent.

For information about the theory behind the discrete phase models, see Discrete Phase in the Theory

Guide. Information is organized into the following sections:

.. Steps for Using the Discrete Phase Models

.. Setting Initial Conditions for the Discrete Phase

.. Setting Boundary Conditions for the Discrete Phase

.. Particle Erosion Coupled with Dynamic Meshes

.. Setting Material Properties for the Discrete Phase

.. Solution Strategies for the Discrete Phase

.. Postprocessing for the Discrete Phase

.. Parallel Processing for the Discrete Phase Model

In addition to solving transport equations for the continuous phase, ANSYS Fluent allows you to simulate

a discrete second phase in a Lagrangian frame of reference. This second phase consists of spherical

particles (which may be taken to represent droplets or bubbles) dispersed in the continuous phase.

ANSYS Fluent computes the trajectories of these discrete phase entities, as well as heat and mass

transfer to/from them. The coupling between the phases and its impact on both the discrete phase

trajectories and the continuous phase flow can be included.

ANSYS Fluent provides the following discrete phase modeling options:

calculation of the discrete phase trajectory using a Lagrangian formulation that includes the discrete phase

inertia, hydrodynamic drag, and the force of gravity, for both steady and unsteady flows

prediction of the effects of turbulence on the dispersion of particles due to turbulent eddies present in the

continuous phase

heating/cooling of the discrete phase

vaporization and boiling of liquid droplets

combusting particles, including volatile evolution and char combustion to simulate coal combustion

optional coupling of the continuous phase flow field prediction to the discrete phase calculations

droplet breakup and coalescence

consideration of particle/particle collisions and voidage of discrete phase

These modeling capabilities allow ANSYS Fluent to simulate a wide range of discrete phase problems

including particle separation and classification, spray drying, aerosol dispersion, bubble stirring of liquids,

liquid fuel combustion, and coal combustion. The physical equations used for these discrete phase

calculations are described in Discrete Phase in the Fluent Theory Guide, and instructions for setup,

solution, and postprocessing are provided in the remaining sections of this chapter.

Alternative models for multiphase systems use the Euler-Euler approach rather than the Euler-Lagrange

approach used in the Discrete Phase Model. The Euler-Euler models are discussed in Modeling Multiphase

Flows (p. ) along with the Dense Discrete Phase Model (DDPM) which is a hybrid Euler-Euler and

Euler-Lagrange approach.

The Lagrangian discrete phase model can be connected to the Eulerian VOF model via VOF-to-DPM

model transfer mechanisms as described in Using the VOF-to-DPM Model Transition for Dispersion of

Liquid in Gas (p. ). For example, in the simulation of liquid sprays, approximately spherical liquid

structures in the VOF solution can be converted automatically into Lagrangian particle parcels. This, in

conjunction with dynamic solution-adaptive mesh refinement, allows for a detailed, yet time-efficient

simulation of primary atomization, such as, for example, in gas turbines and internal combustion engines.

... Concepts

... Limitations

This section introduces several concepts in the treatment of discrete phase particles in Fluent that are

important to understand in order to get the most out of the remaining information in this chapter.

.... Uncoupled vs. Coupled DPM

.... Steady vs. Unsteady Tracking

.... Parcels

When the fluid changes the particles, there will be corresponding effects on the fluid. For example,

when drag force acts on a particle, the exchange of momentum can change the fluid flow. When

simulating particles using DPM, you can choose whether or not to include these effects in the flow

solution; these alternatives are called Coupled and Uncoupled DPM. See Options for Interaction with

the Continuous Phase (p. ) for details about how to specify whether your simulation uses Coupled

or Uncoupled DPM.

In Uncoupled DPM, the only purpose of the DPM particles is for postprocessing, and so particles are

not tracked except when you request them, for example to calculate and display particle tracks. The

particles can still change by heat and mass transfer, but the corresponding changes (such as vapor

from an evaporating droplet) do not affect the flow solution.

In a Coupled DPM simulation, the effects of the particles are used to influence the flow solution. These

effects are transmitted to the flow as DPM Sources. The DPM solution and the flow solution should

reach a converged, self-consistent solution. Therefore, there are several options for running these

solutions together—see Solution Strategies for the Discrete Phase (p. ).

As described in Steps for Using the Discrete Phase Models (p. ), to set up a DPM simulation you

specify the starting conditions of a set of particles by defining an injection. By specifying boundary

conditions and physical sub-models, you also specify how these particles interact with other zones

Modeling Discrete Phase

in the geometry and how they eventually leave the model—for instance, they might bounce off some

walls but be trapped by others.

You must also specify how Fluent is to track the particles you have defined. If Steady Tracking is en-

abled, then, as soon as a particle is released, it is tracked until it reaches its final destination according

to the specified boundary behavior (or until a fixed number of particle time steps have been used).

Therefore, each particle typically travels through many cells of the model, interacting with the flow

and (in a Coupled DPM simulation) changing the DPM Sources in each cell. These sources influence

the flow solution for a defined number of iterations or time steps—the flow solution can be steady

or unsteady. Then, if required, a new set of particle trajectories is tracked, the DPM Sources are updated,

and the sequence is repeated. An example of using Steady DPM with unsteady flow is when the

chosen flow models require a transient simulation, although the final goal is a steady solution.

If Unsteady Tracking is enabled, then each particle is advanced by a specified number of particle time

steps, not necessarily reaching a final destination, before the flow solution is updated. When Unsteady

DPM is coupled to unsteady flow solution, the particles and the flow develop in time together con-

currently, although different time steps can be used for DPM and flow.

Unsteady DPM can also be coupled to steady flow solution; this makes sense if there is a continuous

source of DPM particles that pass through the system. For steady or unsteady flow, there are several

DPM models where Unsteady Tracking is required. For example, in spray coalescence and collision

models, particles change with time on the basis of interactions with other particles, so they must be

tracked simultaneously

Especially when using Coupled DPM, the mass flow rate of a particle injection will often be a required

and relevant input parameter since it determines the absolute value of the DPM Sources. This mass

flow rate could be converted into the number of particles injected per unit time. However, it is often

prohibitive to track that number of particles in a simulation. Strictly speaking, the model therefore

tracks a number of ‘parcels’, and each parcel is representative of a fraction of the total continuous

mass flow rate (in Steady tracking) or a fraction of the total mass flow released in a time step (in Un-

steady tracking).

It is still sometimes helpful to refer to each parcel as a representative particle, because it has a specified

particle diameter, and its trajectory in fluid flow uses the relaxation time appropriate for a single

particle. (The relaxation time is a ratio of particle momentum to drag force). However, the parcel’s

mass (or mass flow rate) becomes important when calculating the DPM Sources: for example, if a

representative droplet loses a small amount of vapor by evaporation, the overall effect from the whole

parcel will typically be much larger. Other models also use the parcel mass (or mass flow rate) to

calculate total concentrations of DPM material—in particular, the Dense Discrete Phase Model (DDPM)

uses this concentration to feed into the volume fraction of the Eulerian phase that represents the

same material. See Dense Discrete Phase Model in the Fluent Theory Guide for details of the Dense

Discrete Phase Model.

The concept of parcels is particularly important in the Discrete Element Method (DEM), where parcels

occupy a finite volume and obstruct other DEM parcels. The volume occupied by a parcel is calculated

directly from the mass that it represents (so that a realistic density is created when parcels pack to-

gether). The equivalent ‘parcel diameter’ is used for calculating parcel-parcel contacts and forces.

However, for trajectories through fluid, it is still the ‘particle diameter’ that is used. See Discrete Element

Method Collision Model in the Fluent Theory Guide for details of the Discrete Element Model.

Introduction

The number of parcels in a DPM model is chosen in the model settings, and not defined by the true

number of particles. There are several inputs that can be used to adjust the number of parcels when

defining initial conditions such as the number of injection locations and (for Unsteady Tracking) the

injection frequency (Setting Initial Conditions for the Discrete Phase (p. )) Other inputs in sub-

models include: the number of sizes in a size distribution (Using the Rosin-Rammler Diameter Distri-

bution Method (p. )); the number of stochastic tries in turbulent dispersion (Specifying Turbulent

Dispersion of Particles (p. )); and the breakup characteristics of some sprays (Breakup (p. )). A

high number of parcels can be computationally expensive, but it is often helpful for convergence, so

that no single parcel has an overwhelming effect on the flow In general you should arrange for enough

parcels to produce a statistical sample, representative of the full range of particle behavior.

The discrete phase model limitations are provided in the following subsections.

.... Limitation on the Particle Volume Fraction

.... Limitation on Modeling Continuous Suspensions of Particles

.... Limitations on Modeling Particle Rotation

.... Limitations on Using the Discrete Phase Model with Other ANSYS Fluent Models

.... Limitations on Using the Hybrid Parallel Method

.... Limitations on Using the Lagrangian Wall Film Model

The discrete phase formulation used by ANSYS Fluent contains the assumption that the second phase

is sufficiently dilute that particle-particle interactions and the effects of the particle volume fraction

on the gas phase are negligible. In practice, these issues imply that the discrete phase must be present

at a fairly low volume fraction, usually less than –%. Note that the mass loading of the discrete

phase may greatly exceed –%: you may solve problems in which the mass flow of the discrete

phase equals or exceeds that of the continuous phase. See Modeling Multiphase Flows (p. ) for

information about when you might want to use one of the general multiphase models instead of the

discrete phase model.

This limitation is relaxed for some variants of DPM. For example, the Dense Discrete Phase Model

(DDPM) adds effects due to friction and volume fraction, so that the concentration can approach the

packing limit. Where high local concentrations of spray droplets cause coalescence and collision,

these phenomena can be included in some spray models. Parcel-parcel contacts between solid particles

are modeled in detail in Discrete Element Models, so that parcels can pack together closely.

The steady-particle Lagrangian discrete phase model is suited for flows in which particle streams are

injected into a continuous phase flow with a well-defined entrance and exit condition. The Lagrangian

model does not effectively model flows in which particles are suspended indefinitely in the continuum,

as occurs in solid suspensions within closed systems such as stirred tanks, mixing vessels, or fluidized

beds. The unsteady-particle discrete phase model, however, is capable of modeling continuous sus-

pensions of particles. See Modeling Multiphase Flows (p. ) for information about when you might

want to use one of the general multiphase models instead of the discrete phase models.

When using rotating particles, note the following limitations:

In simulations with enabled stochastic particle collision models (Including Collision and Droplet Coales-

cence (p. )), particle rotation is not affected by particle/particle collisions.

Particle rotation is not available for massless particles.

Particle rotation is not compatible with moving reference frame simulations.

For atomizer injections, the initial angular velocity is set to zero.

The effect of the Magnus lift force on the fluid is not taken into account in DPM coupled simulations.

.... Limitations on Using the Discrete Phase Model with Other ANSYS Fluent

Models

The following restrictions exist on the use of other models with the discrete phase model:

When tracking particles with the DPM model in combination with any of the multiphase flow

models (VOF, mixture, or Eulerian—see Modeling Multiphase Flows (p. )) the Shared Memory

method cannot be selected (Parallel Processing for the Discrete Phase Model (p. )). (Note that

using the Message Passing or Hybrid method enables the compatibility of all multiphase flow

models with the DPM model.)

When using the DPM model with the Eulerian multiphase model, the tracked particles rely only on the

primary phase to compute drag, heat, and mass transfer. Also, any DPM related source terms are applied

to the primary phase. Particle tracking relative to a secondary phase is not provided.

Streamwise periodic flow (either specified mass flow rate or specified pressure drop) cannot be modeled

with steady particle tracks in coupled simulation. It is possible using transient particle tracks.

Only non-reacting particles can be included when the premixed combustion model is used.

Surface injections will be moved with the mesh when a sliding mesh or a moving or deforming mesh is

being used, however only those surfaces associated with a boundary will be recalculated. Injections from

cut plane surfaces will not be moved with the mesh and will be deleted when remeshing occurs.

The cloud model is not available for unsteady particle tracking, and will not allow you to use the

message passing or hybrid option for the particles.

The wall film model is only valid for liquid materials. If a nonliquid particle interacts with a wall film

boundary, the boundary condition will default to the reflect boundary condition.

When multiple reference frames are used in conjunction with the discrete phase model, the display of

particle tracks will not, by default, be meaningful. Similarly, coupled discrete-phase calculations are not

meaningful.

An alternative approach for particle tracking and coupled discrete-phase calculations with multiple

reference frames is to track particles based on absolute velocity instead of relative velocity. To make

this change, use the define/models/dpm/ options/track-in-absolute-frame text

command. Note that the results may strongly depend on the location of walls inside the multiple

reference frame.

The particle injection velocities (specified in the Set Injection Properties dialog box) are defined

relative to the frame of reference in which the particles are tracked. By default, the injection velo-

cities are specified relative to the local reference frame. If you enable the track-in-absolute-

frame option, the injection velocities are specified relative to the absolute frame.

Relative particle tracking cannot be used in combination with sliding and moving deforming meshes. If

sliding and/or deforming meshes are used with the DPM model, the particles will always be tracked in

the absolute frame. Switching to the relative frame is not permitted.

The hybrid parallel DPM tracking method is not available with the following models and features:

– the PDF Transport model

– the DDPM (Dense DPM) model with the Volume Fraction Approaching Packing Limit option selected

in the Discrete Phase dialog box

– the Stochastic Collision model (with or without the droplet coalescence)

– Graphical display of particle tracks

– Sampling of particle tracks in sample files

– Export of particle tracks into particle history files

If any of these models or features are used, Fluent will silently fall back to the Message Passing

parallel DPM tracking option.

The Use DPM Domain option of the Hybrid parallel DPM tracking method will not be used in any

of the following situations:

– if the Eulerian Wall Film model is enabled

– if the PDF Transport model is enabled

– if the case has a dynamic zone

– if the case has a sliding interface

– if the case includes non-zonal surface injections (that is, injections that have positions defined through

surfaces that are not zone surfaces)

If the Use DPM Domain option is enabled in such cases, ANSYS Fluent will issue a message warning

that the DPM Domain is suppressed. You can avoid this message by disabling the Use DPM Domain

option in the Parallel tab of the Discrete Phase Model dialog box.

For additional limitations associated with the hybrid parallel method, see Limitations on Using the

Discrete Phase Model with Other ANSYS Fluent Models (p. ).

The Lagrangian wall film model is only available with Unsteady Particle Tracking.

The Lagrangian wall film model is not compatible with hanging node mesh refinement on walls.Though

the fluid meshes can be adapted, the refined meshes must not touch walls where the wall film model is

enabled.

The wall film model assumes liquid particle materials. If an inert particle interacts with a wall film boundary,

it is assumed to be liquid for the wall film model calculations. For combusting particles, the wall film is

applied if Wet Combustion Model is enabled and as long as the liquid fraction in the particle is nonzero.

If a dry combusting particle interacts with a wall film boundary it will stick to the wall and follow the

combusting particle laws.

The wall film model is not compatible with the Rosseland Radiation model.

The Workpile Algorithm option is not available with the wall film boundary condition. It will be disabled

automatically when choosing to simulate a wall film on a wall.

For additional assumptions used by the Lagrangian wall film model, refer to Introduction and Interaction

During Impact with a Boundary in the Fluent Theory Guide.

You can include a discrete phase in your ANSYS Fluent model by defining the initial position, velocity,

size, and temperature of individual particles. These initial conditions, along with your inputs defining

the physical properties of the discrete phase, are used to initiate trajectory and heat/mass transfer cal-

culations. The trajectory and heat/mass transfer calculations are based on the force balance on the

particle and on the convective/radiative heat and mass transfer from the particle, using the local con-

tinuous phase conditions as the particle moves through the flow. The predicted trajectories and the

associated heat and mass transfer can be viewed graphically and/or alphanumerically.

The procedure for setting up and solving a problem involving a discrete phase is outlined below, and

described in detail in Options for Interaction with the Continuous Phase (p. ) – Postprocessing for

the Discrete Phase (p. ). Only the steps related specifically to discrete phase modeling are shown

here. For information about inputs related to other models that you are using in conjunction with the

discrete phase models, see the appropriate sections for those models.

. Enable any of the discrete phase modeling options, if relevant, as described in Options for Interaction with

the Continuous Phase (p. ).

. Choose a transient or steady treatment of particles as described in Steady/Transient Treatment of

Particles (p. ).

. Specify tracking parameters as described in Tracking Parameters for the Discrete Phase Model (p. ).

. Enable the required physical submodels for the discrete phase model, as described in Physical Models for

the Discrete Phase Model (p. ).

. Set the numerics parameters and solve the problem, as described in Numerics of the Discrete Phase Mod-

el (p. ) and Solution Strategies for the Discrete Phase (p. ).

. Specify the injection-specific models, initial conditions, and particle size distributions as described in Setting

Initial Conditions for the Discrete Phase (p. ).

. Initialize the flow field.

. Solve the coupled or uncoupled flow (Solution Strategies for the Discrete Phase (p. )).

Steps for Using the Discrete Phase Models

. For transient cases, advance the solution in time by taking the desired number of time steps. Particle pos-

itions will be updated as the solution advances in time. If you are solving an uncoupled flow, the particle

position will be updated at the end of each time step. For a coupled calculation, the positions are iterated

on or within each time step.

... Options for Interaction with the Continuous Phase

If the discrete phase interacts (that is, exchanges mass, momentum, and/or energy) with the continuous

phase, you should enable Interaction with Continuous Phase.

Setup → Models → Discrete Phase

Continuous Phase Interaction → On

An input for the DPM Iteration Interval will appear, which allows you to control the frequency at

which the particles are tracked and the DPM sources are updated.

For steady-state simulations, increasing the DPM Iteration Interval will increase stability but require

more iterations to converge.

In addition, another option exists that allows you to control the numerical treatment of the source

terms and how they are applied to the continuous phase equations. For unsteady simulations, Update

DPM Sources Every Flow Iteration is the default (and recommended) option; at every DPM Iteration,

the particle source terms are recalculated. The source terms applied to the continuous phase equations

transition to the new values every flow iteration based on Equation . to Equation . in the

Theory Guide. This process is controlled by the under-relaxation factor, specified in the Solution

Controls task page, see Under-Relaxation of the Interphase Exchange Terms (p. ).

... Steady/Transient Treatment of Particles

The Discrete Phase Model uses a Lagrangian approach to derive the equations for the underlying

physics, which are solved transiently. Transient numerical procedures in the Discrete Phase Model can

be applied to resolve steady flow simulations as well as transient flows.

In the Discrete Phase Model Dialog Box (p. ) you have the option of choosing whether you want to

treat the particles in an unsteady or a steady fashion. This option can be chosen independent of the

settings for the solver. Thus, you can perform steady-state trajectory simulations even when selecting

a transient solver for numerical reasons. You can also specify unsteady particle tracking when solving

the steady continuous phase equations. This can be used to improve numerical stability for very large

particle source terms or simply for postprocessing purposes. Whenever you enable a breakup or collision

model to simulate sprays, the Unsteady Particle Tracking will be switched on automatically.

When Unsteady Particle Tracking is enabled, several new options appear. If steady-state equations

are solved for the continuous phase, you simply enter the Particle Time Step Size and the Number

of Time Steps, thus tracking particles every time a DPM iteration is conducted. When you increase

the Number of Time Steps, the droplets penetrate the domain faster.

When solving unsteady equations for the continuous phase, you must decide whether you want to

use Fluid Flow Time Step to inject the particles, or you prefer a Particle Time Step Size independent

of the Fluid Flow Time Step. With the latter option, you can use the Discrete Phase Model in combin-

ation with changes in the time step for the continuous equations, as it is done when using adaptive

flow time stepping.

If you do not use Fluid Flow Time Step, you must decide when to inject the particles for a new time

step. You can either Inject Particles at Particle Time Step or at the Fluid Flow Time Step. In any

case, the particles will always be tracked in such a way that they coincide with the flow time of the

continuous flow solver, as long as the maximum number of time steps used to compute a single tra-

jectory is sufficient (see Tracking Parameters for the Discrete Phase Model (p. ) for details).

You can use a user-defined function (DEFINE_DPM_TIMESTEP) to change the time step for DPM

particle tracking. The time step can be prescribed for special applications where a certain time step is

needed. For more information about changing the time step size for DPM particle tracking, see

DEFINE_DPM_TIMESTEP in the Fluent Customization Manual.

Important

When the density-based solver is used with the explicit unsteady formulation, the particles

are advanced once per time step and are calculated at the start of the time step (before

the flow is updated).

Additional inputs are required for each injection in the Set Injection Properties Dialog Box (p. ), as

detailed in Defining Injection Properties (p. ). For Unsteady Particle Tracking, the injection Start

Time and Stop Time must be specified under Point Properties. Injections with start and stop times

set to zero will be injected only at the start of the calculation (

). If the In-Cylinder mesh motion is

enabled, the start and stop times are replaced by Start Crank Angle and Stop Crank Angle, respectively.

The injection specified in this way will be repeated at the starting and stopping crank angle if the

simulation is run through more than one cycle. Changing injection settings during a transient simulation

will not affect particles currently released in the domain. At any point during a simulation, you can

clear particles that are currently in the domain by clicking the Clear Particles button in the Discrete

Phase Model Dialog Box (p. ).

You can choose the Parcel Release Method to determine how ANSYS Fluent creates parcels. For an

overview of the concept of parcels, see Parcels (p. ). The methods available are:

standard

injects a single parcel per injection stream per time step.The number of particles in the parcel,

, is

determined as follows:

(.)

where,

is the number of particles in a parcel

is the mass flow rate of the particle stream

is the time step

is the particle mass

This is the default method.

constant-number

injects parcels with a user-specified number of particles per parcel.The number of parcels is determined

to satisfy the specified mass-flow rate and particle size distribution for the injection.

constant-mass

injects parcels with a user-specified parcel mass.The number of parcels is determined to satisfy the specified

mass-flow rate and particle size distribution for the injection.

constant-diameter

injects parcels with a user-specified parcel diameter.The number of parcels is determined to satisfy the

specified mass-flow rate and particle size distribution for the injection.

Note that for atomizer injections, file injections, or injections that use the DEFINE_DPM_INJEC-

TION_INIT user defined function, the Fluent solver automatically uses the default standard parcel

release method. Other parcel release methods are not available.

For cases involving sprays and particle size distributions in general, the recommended setting for

Parcel Release Method is constant-number. For DEM simulations, you can use constant-diameter

or constant-mass to ensure that the parcel diameter does not exceed the size of the smallest cells in

the computational mesh.

Note that a lower value specified for constant-number, constant-mass, or constant-diameter will

result in a larger number of parcels injected and a finer discretization of the DPM phase. This may be

beneficial for accuracy and stability of the calculation, at the expense of additional computational cost.

The Parcel Release Method is specified in the Parcel tab of the Set Injection Properties dialog box.

You can also choose one of several methods to control when the particles are tracked.

In steady-state simulations, particles are tracked at the user-specified intervals (DPM Iteration Interval).

Individual particles are tracked from their injection position until either they escape the domain or certain

termination criteria are met. Particle tracking is performed only if the global Number of Iterations is equal

to or exceeds DPM Iteration Interval.The particle sources are updated during tracking, and then applied

to the gas phase in subsequent flow iterations.

In transient flow simulations, particle tracking always occurs at the beginning of each flow time step, irre-

spective of DPM Iteration Interval.The particles are advanced in time based on the current continuous-

phase solution, and DPM sources are updated.The DPM sources prevail up to the next time the particle

tracker is run.

(transient flow) If the DPM Iteration Interval is larger than or equal to Max Iterations/Time Step, then

particles are tracked only once per time step. If the DPM Iteration Interval is less than Max Iterations/Time

Step, then the particle tracker is run multiple times during the time step. Each time the particle tracker is

used, particles are returned to their original state at the beginning of the time step.Then particles are ad-

vanced in time based on the current continuous-phase solution, and DPM sources are updated. If Particle

Time Step is larger than Fluid Flow Time Step (to allow injection of particles at a different time scale than

the fluid), then particles are advanced only for the fluid flow time step.

(transient flow) If you specify a value of zero as the DPM Iteration Interval, the particles are advanced at

the end of the time step. Note that if you have previously enabled the resetting of DPM source terms at

the beginning of every time step using the TUI command define/models/dpm/interaction/reset-

sources-at-timestep?, ANSYS Fluent will disable this option once you set the DPM Iteration Interval

to zero, because this feature combination is not advisable.

In cases where Interaction with Continuous Phase is enabled, you must provide a sufficient number

of particle source term updates to ensure that particle source terms reach their final values (see Fig-

ure . : Effect of Number of Source Term Updates on Source Term Applied to Flow Equations (p. )).

This can be achieved either by setting the DPM under-relaxation factor to  or in other cases by enabling

Update DPM Sources Every Flow Iteration. If the latter is disabled and the DPM under-relaxation

factor is less than , then the value you specify for DPM Iteration Interval must be small compared

to Max Iterations/Time Step.

Important

In steady-state discrete phase modeling, particles do not interact with each other and are tracked

one at a time in the domain.

If the collision model is used, you will not be able to set the DPM Iteration Interval. Refer to

Collision and Droplet Coalescence Model Theory in the Fluent Theory Guide for details about this

limitation.

Note

As explained in Setting Initial Conditions for the Discrete Phase (p. ), the injection flow

rate is defined per unit meter of depth in 2D problems. In such cases, each injected parcel

is considered to be a solid cylinder of diameter

and depth  meter. The parcel volume

is then expressed as:

However, the particles that are dense-packed in the parcel are assumed to be spheres rather

than pucks (ice-hockey). The volume of each particle is the same as in 3D cases:

Consider next the theoretical atomic packing factor  of spherical particles in a cylinder of

one meter depth, also expressed as the volume ratio of all particles to all injected parcels.

In 2D, the particles of diameter

are stacked on top of one another in a cylinder of dia-

meter

and depth  meter. The total number of particles that can be stacked in the cylinder

in such a way is

. The total volume occupied by these particles is

The volume of the surrounding parcel cylinder of depth  m is

The atomic packing factor  will have a constant value of / when expressed as:

In order to use the same parameters (spring constant  and coefficient of restitution ) for

the DEM spring dashpot models in both 3D and 2D simulations, parcels of the same mass

must be injected in 3D and 2D.

In 3D, the injected parcel is a sphere with diameter

and mass

. The

number of spherical particles in a spherical parcel is calculated by

In 2D, the parcel is a cylinder of  m depth. This cylinder has the same mass as the spherical

parcel in 3D (

), but its volume differs and is calculated as:

The number of particles per cylindrical parcel NP and the volume they occupy is the same

as in 3D, that is

Since the ratio of these two volumes must be equal to the theoretical atomic packing factor

, we obtain

The parcel diameter in 2D can then be calculated as:

Note that in 2D, the parcel diameter

is used as a collision range and it is different than

the parcel diameter

in 3D.

For each parcel release method, the input values for the parcel mass and parcel diameter

(

and

, respectively) are the same in both 3D and 2D, while the output values for

in 3D.

(

and

parcel diameters are different:

in 2D simulations and

in 3D simulations.

...Tracking Parameters for the Discrete Phase Model

You will use two parameters to control the time integration of the particle trajectory equations:

the maximum number of time steps

This factor is used to abort trajectory calculations when the particle never exits the flow domain.

the length scale/step length factor

This factor is used to set the time step for integration within each control volume.

Each of these parameters is set in the Discrete Phase Model Dialog Box (p. ) (Figure . : The Discrete

Phase Model Dialog Box and the Tracking Parameters (p. )) under Tracking Parameters in the

Tracking tab.

Edit...

Figure . : The Discrete Phase Model Dialog Box and the Tracking Parameters

Max. Number of Steps

is the maximum number of time steps used to compute a single particle trajectory via integration of

Equation . in the Theory Guide.When the maximum number of steps is exceeded, ANSYS Fluent

abandons the trajectory calculation for the current particle injection and reports the trajectory fate as

“incomplete”.The limit on the number of integration time steps eliminates the possibility of a particle

being caught in a recirculating region of the continuous phase flow field and being tracked infinitely.The

default value for this parameter is , for steady-state particle tracking and  for unsteady particle

tracking. Note that you may easily create problems in which the default value is insufficient for completion

of the trajectory calculation. In this case, when trajectories are reported as incomplete within the domain

and the particles are not recirculating indefinitely, you can increase the maximum number of steps (up

to a limit of

).

Note

If, when opening a previous simulation with unsteady DPM particle tracking, you receive

a warning reporting that a fraction of the discrete phase mass is "behind in time", you

can use the reported percentage values to determine if it is a significant enough discrep-

ancy to warrant revising the simulation to have a higher value for Max. Number of

Steps.

Length Scale

controls the integration time step size used to integrate the equations of motion for the particle.The in-

tegration time step is computed by ANSYS Fluent based on a specified length scale , and the velocity

of the particle (

) and of the continuous phase (

):

(.)

where  is the Length Scale that you define. As defined by Equation . (p. ),

is proportional

to the integration time step and is equivalent to the distance that the particle will travel before

its motion equations are solved again and its trajectory is updated. A smaller value for the Length

Scale increases the accuracy of the trajectory and heat/mass transfer calculations for the discrete

phase.

(Note that particle positions are always computed when particles enter/leave a cell; even if you

specify a very large length scale, the time step used for integration will be such that the cell is

traversed in one step.)

Length Scale will appear in the Discrete Phase Model dialog box when the Specify Length Scale

Step Length Factor

also controls the time step size used to integrate the equations of motion for the particle. It differs from

the Length Scale in that it allows ANSYS Fluent to compute the time step in terms of the number of time

steps required for a particle to traverse a computational cell.To set this parameter instead of the Length

Scale, turn off the Specify Length Scale option.

The integration time step is computed by ANSYS Fluent based on a characteristic time that is related

to an estimate of the time required for the particle to traverse the current continuous phase control

volume. If this estimated transit time is defined as

, ANSYS Fluent chooses a time step

as

(.)

where  is the Step Length Factor. As defined by Equation . (p. ),

is inversely proportional

to the integration time step and is roughly equivalent to the number of time steps required to

traverse the current continuous phase control volume. A larger value for the Step Length Factor

decreases the discrete phase integration time step. The default value for the Step Length Factor

is . Step Length Factor will appear in the Discrete Phase Model dialog box when the Specify

Length Scale option is off (the default setting).

For steady-state particle tracking, one simple general rule to follow when setting the parameters above

is that if you want the particles to advance through a domain consisting of

mesh cells into the main

flow direction, the Step Length Factor times

should be approximately equal to the Max. Number

of Steps.

When Accuracy Control is enabled in the Numerics tab, the settings for Step Length Factor and

Length Scale will be used only to estimate the time step of the first integration step. In all subsequent

integration steps, the particle integration time step is adapted to achieve the tolerance specified in

Numerics of the Discrete Phase Model (p. ).

... Drag Laws

There are eight drag laws for the particles that can be selected for each injection. These are specified

on the Physical Models tab of the Set Injection Properties dialog box. See Specifying Injection-

Specific Physical Models (p. ) for details.

... Physical Models for the Discrete Phase Model

This section provides instructions for using the optional discrete phase models available in ANSYS

Fluent. All of them can be enabled in the Physical Models tab of the Discrete Phase Model dialog

box (Figure . : The Discrete Phase Model Dialog Box and the Physical Models (p. )).

Edit...

Figure . : The Discrete Phase Model Dialog Box and the Physical Models

.... Including Radiation Heat Transfer Effects on the Particles

If you want to include the effect of radiation heat transfer to the particles (Equation . in the Theory

Guide), you must enable the Particle Radiation Interaction option under the Physical Models tab,

in the Discrete Phase Model Dialog Box (p. ) (Figure . : The Discrete Phase Model Dialog Box and

the Physical Models (p. )). You also must define additional properties for the particle materials

(emissivity and scattering factor), as described in Description of the Properties (p. ). This option is

available only when the P- or discrete ordinates radiation model is used.

.... Including Thermophoretic Force Effects on the Particles

If you want to include the effect of the thermophoretic force on the particle trajectories (Equation .

in the Theory Guide), enable the Thermophoretic Force option under the Physical Models tab, in

the Discrete Phase Model Dialog Box (p. ). You also must define the thermophoretic coefficient for

the particle material, as described in Description of the Properties (p. ).

.... Including Saffman Lift Force Effects on the Particles

For sub-micron particles, you can also model the lift due to shear (the Saffman lift force, described

in Saffman’s Lift Force in the Theory Guide) in the particle trajectory. To do this, enable the Saffman

Lift Force option under the Physical Models tab, in the Discrete Phase Model Dialog Box (p. ).

.... Including the Virtual Mass Force and Pressure Gradient Effects on Particles

In cases where the density of the fluid approaches or exceeds the density of the particles (for example

liquid flow with gaseous bubbles), it is recommended that you include the Virtual Mass and Pressure

Gradient forces in the particle force balance. To do this, enable Virtual Mass Force and Pressure

Gradient Force under the Physical Models tab in the Discrete Phase Model Dialog Box (p. ). See

Other Forces in Fluent Theory Guide for information on the Virtual Mass and Pressure Gradient forces.

.... Monitoring Erosion/Accretion of Particles at Walls

To monitor particle erosion and accretion rates at wall boundaries:

. Enable Erosion/Accretion in the Physical Models tab of the Discrete Phase Model Dialog Box (p. ).

Enabling the Erosion/Accretion option will cause the erosion and accretion rates to be calculated

at wall boundary faces when particle tracks are updated.

. For each wall zone, select erosion models and specify erosion model parameters as described in Setting

Particle Erosion and Accretion Parameters (p. ).

. If you want to couple particle erosion with dynamic meshes to account for changes in the shape and

position of eroded walls, follow the procedure described in Particle Erosion Coupled with Dynamic

Meshes (p. ).

.... Pressure Options for Vaporization Models

You can use the text interface command

define/models/dpm/options/use-absolute-pressure-for-vaporization?

to select whether the absolute pressure or a constant Operating Pressure (set in the Operating

Conditions dialog box) is used in the vaporization rate calculations.

The default and recommended setting is to use the absolute pressure. However, in some incompressible

flow cases, when there are large pressure variations in the droplet injection region, selecting the

constant operating pressure may stabilize the solution.

See Operating Pressure, Gauge Pressure, and Absolute Pressure (p. ) and Equation . (p. ) for

definitions of the operating pressure and absolute pressure.

.... Enabling Pressure Dependent Boiling

With this option you can modify the condition for switching from droplet vaporization (Law ) to

boiling (Law ). By default ANSYS Fluent will switch from the vaporization to the boiling law when

the particle temperature has reached the boiling point defined for the droplet material (Equation .

in the Theory Guide). When the Pressure Dependent Boiling option is enabled, the switching condition

will change to

, where

is the saturation vapor pressure at the droplet temperature and

is the domain pressure. If

while in the boiling law, the model will switch back to the vaporiz-

ation law. If this option is enabled it is essential to enter the appropriate droplet saturation vapor

pressure data to cover the complete pressure/temperature range in your model.

When Pressure Dependent Boiling is enabled, then the Temperature Dependent Latent Heat

model automatically applies (see Including the Effect of Droplet Temperature on Latent Heat (p. )).

Setting the Pressure Dependent Boiling option has no effect on the multicomponent particles,

where switching from the vaporization to the boiling regime is always based on the component sat-

uration vapor pressures (see Multicomponent Particle Definition (Law ) in the Theory Guide).

In the supercritical pressure regime, failure of the saturation temperature calculation algorithm may

indicate that the multicomponent droplet has approached the critical temperature, provided that

you have entered accurate vapor pressure data for all components. In such a case, you can use the

failure?

failure?

When this option is enabled, ANSYS Fluent dumps the particle mass into the continuous phase if the

saturation temperature calculation fails.

Finally, selection of the Pressure Dependent Boiling option is not available with the real-gas models,

as the pressure dependence always applies. See Using the Cubic Equation of State Models with the

Lagrangian Dispersed Phase Models (p. ) for more information.

For pressures higher than the critical pressure of the droplet material (

), a boiling point

,

defined as the temperature at the saturation vapor pressure (

), cannot be determined as the

vapor pressure curve is defined only up to the critical point. Under supercritical pressure conditions

(

), the vaporization models are applicable at droplet temperatures below the critical point (

),

and the switching condition from vaporization to boiling is never met. For supercritical pressure

conditions, you must enter the droplet saturation vapor pressure data for the complete pressure/tem-

perature range up to the critical point

.

When Pressure Dependent Boiling is enabled, you can use the text user interface command

/define/models/dpm/options/allow-supercritical-pressure-vaporization?

to enforce the switching from vaporization to boiling even if the boiling point

is not calculated

from the vapor pressure data.

If the pressure in your model is above critical (

), you must retain the default setting (yes) for

allow-supercritical-pressure-vaporization?.

For subcritical pressure conditions (

), the setting for allow-supercritical-pressure-

vaporization? will have no effect unless the boiling point calculation fails, which usually indicates

that either the vapor pressure data do not cover the complete temperature/pressure range for your

model, or inaccurate data have been entered. In that case, if allow-supercritical-pressure-

vaporization? is set to no, the normal boiling point

defined for the droplet material will be

imposed as a switching condition from vaporization to boiling.

.... Including the Effect of Droplet Temperature on Latent Heat

To include the droplet temperature effects on the latent heat as described in Equation . in the

Theory Guide, enable Temperature Dependent Latent Heat under the Physical Models tab. If you

enable this option you must provide accurate temperature-dependent specific heat data for both the

droplet and the evaporating species materials.

.... Including the Effect of Particles on Turbulent Quantities

Particles can damp or produce turbulent eddies [] (p. ). In ANSYS Fluent, the formulation described

in [] (p. ) and [] (p. ) is used to compute turbulence modulation. Damping occurs when the

particle diameter is less than one tenth of the turbulent length scale. For larger particle diameters

turbulence kinetic energy is produced [] (p. ).

If you want to consider these effects in the chosen turbulence model, you can enable this using Two-

Way Turbulence Coupling, under the Physical Models tab.

.... Including Collision and Droplet Coalescence

To include the effect of collisions, as described in Collision and Droplet Coalescence Model Theory in

the Theory Guide, select Stochastic Collision and Coalescence under Options.

Note

Coalescence will appear under Options after Stochastic Collision has been enabled.

.... Including the DEM Collision Model

The DEM collision model is suitable for simulating granular matter, where such simulations are char-

acterized by a high volume fraction of particles, and the particle-particle interaction is important. See

Modeling Collision Using the DEM Model (p. ) for details about using this model.

.... Including Droplet Breakup

To model droplet breakup in ANSYS Fluent, enable Breakup under Options. By default, this will enable

Consider Children in the Same Tracking Step and breakup for all suitable injections. You can then

specify the breakup models and parameters (or disable breakup) for each individual injection on the

Physical Models tab in the Set Injection Properties dialog box as described in Breakup (p. ).

The Consider Children in the Same Tracking Step option collects newly generated child droplets

and track them within the same time step. It provides higher accuracy and can lead to faster conver-

gence within a transient flow time step. This option is also automatically enabled if you select wall-

film as Boundary Cond. Type in the Wall dialog box (DPM tab).

.... Modeling Collision Using the DEM Model

To enable the DEM collision model, select DEM Collision under Options. A detailed description of

this model can be found in Discrete Element Method Collision Model in the Theory Guide.

. In the Physical Models tab of the Discrete Phase Model dialog box

Figure . : Discrete Phase Dialog Box with DEM Collision Model

a.

Specify the settings your model requires under DEM Collision Model.

b. (Optional) By default, Adaptive Collision Mesh Width is enabled.This adjusts the width of the collision

mesh to the largest parcel diameter multiplied by the Edge Scale Factor. If Adaptive Collision Mesh

Width is disabled, a fixed Static Collision Mesh Width has to be given in the chosen units of length.

c.

The Maximum Particle Velocity limits the maximum particle velocity to a physically plausible range.

. Set up the injection.

Setup → Models → Discrete Phase → Injections

New...

a.

In the Set Injection Properties dialog box, select a name from the DEM Collision Partner drop-

down list that will serve as the collision partner. A default name using the particle material will be

suggested.

Note

Selecting none from the drop-down list indicates that the particles released from

this injection do not participate in the DEM collision computation.

b. If you want to use the rolling friction collision law (see step ), under the Physical Models tab, enable

Particle Rotation for those injections whose particles take part in collisions with rolling friction.

. Set the boundary conditions for the discrete phase as you normally would. If the Boundary Cond.Type

is reflect, select a name from the DEM Collision Partner drop-down list to designate the collision partner

For example, in Figure . :Wall Boundary Condition for the DEM Model (p. ), a wall boundary condition

will suggest a wall material name, which will designate the collision partner.The name will have a dem-

prefix However, if the DEM Collision Partner is none, the wall will reflect particles like any other DPM

particles using the settings for the Discrete Phase Reflection Coefficients in the Normal and Tangent

directions.These settings generally apply for particles that are not colliding according to DEM, such as

massless particles.

Figure . : Wall Boundary Condition for the DEM Model

. Define the particle interaction between the pairs of the collision partners.

a.

Click the DEM Collisions... button at the bottom of the Discrete Phase Model dialog box.The DEM

Collisions dialog box (Figure . : Collision Dialog Box (p. )) will appear where you can manage

the collision partners.You can Create, Copy, Rename, Delete, and List collision partners.To define

collision laws for a collision partner, select a collision partner from the Collision Partners list and

click the Set... button, or simply double-click the collision partner in the list.

Figure . : Collision Dialog Box

b. In the DEM Collision Settings dialog box (Figure . : DEM Collision Settings Dialog Box (p. )), a

list of all the possible Collision Pairs will exist.

Figure . : DEM Collision Settings Dialog Box

i.

Select a pair of collision partners from the Collision Pairs list.

ii.

For this pair, select the Contact Force Laws that best describe the collision between these two

partners.

The Normal contact force laws that exist are:

spring

spring-dashpot

hertzian

hertzian-dashpot

partners.

spring

hertzian

You can also choose to exclude the contact force law by selecting none.

For the Tangential contact force law (if considered), you can select form the following

friction collision laws:

friction-dshf

friction-dshf-rolling (an extension of the friction-dshf friction collision law including rolling

friction)

Each of the laws is described in the following sections:

The Spring Collision Law in the Fluent Theory Guide

The Spring-Dashpot Collision Law in the Fluent Theory Guide

The Hertzian Collision Law in the Fluent Theory Guide

The Hertzian-Dashpot Collision Law in the Fluent Theory Guide

The Friction Collision Law in the Fluent Theory Guide

Rolling Friction Collision Law for DEM in the Fluent Theory Guide

iii. Enter the Constants for the chosen Contact Force Laws. Refer to Theory in the Theory Guide for

guidance on how to find reasonable values of the force-law constants.

iv. Repeat for all other collision pairs.

v.

Click OK or Apply to apply these settings.

Note

The choice of collision laws does not depend on the order in the pair of collision partners.

Failing to specify a force law for a collision pair implies that respective particles will not collide.

Rolling friction will only be factored in for a particular DEM particle injection if the Particle

Rotation option is selected in the Set Injection Properties dialog box (Physical Properties

tab).

Note

For parallel calculations, the DEM collision model can be optimized by enabling the hybrid

optimization method for DPM. This method balances the load across machines, and,

tab).

Note

within each machine, the hybrid parallel DPM method is used to make sure the load is

balanced by multi-threading. For more information, see the description of the Hybrid

Optimization option in the Weighting tab discussion in Partitioning (p. ).

..... Limitations

The following limitations currently apply when using the DEM collision model:

Axisymmetric geometry cannot be used.

Dynamic mesh motion cannot be used.

The Eulerian wall film model cannot be used.

Shear stress boundary conditions cannot be used at walls.

Marangoni stress boundary condition cannot be used at walls.

DEM particles do not transfer heat from particle to particle during contact.

..... Numeric Recommendations

To better preserve energy during particle collision, the following settings in the Numerics tab are

recommended and will be automatically set when DEM Collisions are enabled.

. Disable Accuracy Control to ensure that DEM time stepping remains small.

. Disable Automated under Tracking Scheme Selection.

. Select implicit from the Tracking Scheme drop-down list.

Refer to Numerics for Tracking of the Particles (p. ) for more information about the settings in the

Numerics tab.

... User-Defined Functions

User-defined functions can be used to customize the discrete phase model to include additional body

forces, modify interphase exchange terms (sources), calculate or integrate scalar values along the

particle trajectory, and incorporate nonstandard erosion rate definitions. More information about user-

defined functions can be found in the Fluent Customization Manual.

Figure . : The Discrete Phase Model Dialog Box and the UDFs

In the Discrete Phase Model Dialog Box (p. ), under User-Defined Functions in the UDF tab, there

are drop-down lists labeled (see Figure . : The Discrete Phase Model Dialog Box and the UDFs (p. )):

Body Force

Scalar Update

Source

Spray Collide Function

DPM Time Step

Erosion/Accretion (if Erosion/Accretion is enabled under the Physical Models tab)

Impingement Model, Film Regime and Splashing Distribution (if either wall-film is selected for

Boundary Cond.Type in the DPM tab of the Wall dialog box or the Eulerian Wall Film model is enabled).

Note that user-defined Impingement Model and Splashing Distribution will overwrite the impinge-

ment/splashing model selected for the Lagrangian or Eulerian wall film boundary condition.

These lists will show available user-defined functions that can be selected to customize the discrete

phase model (see Fluent Customization Manual for more information).

In addition, you can specify a Number of Scalars which are allocated to each particle and can be used

to store information when implementing your own particle models.

... Numerics of the Discrete Phase Model

The underlying physics of the Discrete Phase Model is described by ordinary differential equations

(ODE) as opposed to the continuous flow which is expressed in the form of partial differential equations

(PDE). Therefore, the Discrete Phase Model uses its own numerical mechanisms and discretization

schemes, which are completely different from other numerics used in ANSYS Fluent.

Figure . : The Discrete Phase Model Dialog Box and the Numerics

The Numerics tab gives you control over the numerical schemes for particle tracking as well as solutions

of heat and mass equations (Figure . : The Discrete Phase Model Dialog Box and the Numerics (p. )).

.... Numerics for Tracking of the Particles

To solve equations of motion for the particles, the following numerical schemes are available:

implicit

uses an implicit Euler integration of Equation . in the Theory Guide which is unconditionally stable

for all particle relaxation times.

trapezoidal

uses a semi-implicit trapezoidal integration.

analytic

uses an analytical integration of Equation . of the Theory Guide where the forces are held constant

during the integration.

runge-kutta

facilitates a 5th order Runge Kutta scheme derived by Cash and Karp  [] (p. ).

For additional details, see Solution Strategies for the Discrete Phase (p. ).

You can either choose a single tracking scheme, or switch between higher order and lower order

tracking schemes using an automated selection based on the accuracy to be achieved and the stability

range of each scheme. In addition, you can control how accurately the equations need to be solved.

Accuracy Control

enables the solution of equations of motion within a specified tolerance.This is done by computing the

error of the integration step and reducing the integration step if the error is too large. If the error is

within the given tolerance, the integration step will also be increased in the next steps.

Tolerance

is the maximum relative error that has to be achieved by the tracking procedure. Based on the numerical

scheme, different methods are used to estimate the relative error.The implemented Runge-Kutta scheme

uses an embedded error control mechanism.The error of the other schemes is computed by comparing

the result of the integration step with the outcome of a two step procedure with half the step size.

Max. Refinements

is the maximum number of step size refinements in one single integration step. If this number is exceeded

the integration will be conducted with the last refined integration step size.

Automated Tracking Scheme Selection

provides a mechanism to switch in an automated fashion between numerically stable lower order

schemes and higher order schemes, which are stable only in a limited range. In situations where the

particle is far from hydrodynamic equilibrium, an accurate solution can be achieved very quickly with a

higher order scheme, since these schemes need less step refinements for a certain tolerance.When the

particle reaches hydrodynamic equilibrium, the higher order schemes become inefficient since their

step length is limited to a stable range. In this case, the mechanism switches to a stable lower order

scheme and facilitates larger integration steps.

Important

This mechanism is only available when Accuracy Control is enabled.

High Order Scheme

can be chosen from the group consisting of trapezoidal and runge-kutta scheme.

Low Order Scheme

consists of implicit and the exponential analytic integration scheme.

Tracking Scheme

is selectable only if Automated is switched off.You can choose any of the tracking schemes.You also

can combine each of the tracking schemes with Accuracy Control.

Note

When DEM Collisions are enabled, ANSYS Fluent will automatically set Tracking Scheme to

implicit and disable Accuracy Control.

The equation for rotating particle motion (Equation . in the Fluent Theory Guide) is solved

using the Euler implicit discretization scheme.

.... Including Coupled Heat-Mass Solution Effects on the Particles

By default, the particle heat and mass equations are solved in a segregated manner using an implicit

Euler integration over the time step used for the trajectory calculation If you enable the Coupled

Heat-Mass Solution option for the Droplet, Combusting, or Multicomponent particles, ANSYS

Fluent will solve the corresponding equations using a coupled ODE solver with error tolerance control.

The increased accuracy, however, comes at the expense of increased computational time.

To ensure solution accuracy for the Droplet and Multicomponent particles, ANSYS Fluent will auto-

matically switch to the coupled algorithm during the integration time step when the evaporated

mass is greater than the limiting mass change

(defined in Equation . (p. )), or when the

particle temperature change is greater than the limiting temperature change

(defined in Equa-

tion . (p. )).

(.)

where

is the particle mass (kg) and

is the vaporization limiting factor for the mass.

(.)

where

is the particle temperature (K),

(.)

where

(.)

where

is the bulk temperature (K), and

is the vaporization

limiting factor for the temperature.

You will enter the Vaporization Limiting Factors for Mass

and Heat

. The default values of

. and . have been determined by systematic testing and are recommended for computations.

....Tracking in a Reference Frame

Particle tracking is related to a coordinate system. With Track in Absolute Frame enabled, you can

choose to track the particles in the absolute reference frame. All particle coordinates and velocities

are then computed in this frame. The forces due to friction with the continuous phase are transformed

to this frame automatically.

In rotating flows it might be appropriate for numerical reasons to track the particles in the relative

reference frame. If several reference frames exist in one simulation, then the particle velocities are

transformed to each reference frame when they enter the fluid zone associated with this reference

frame.

When the impact of particles with walls in multiple rotating reference frames is important, as it is the

case with a rotating impeller in a stationary baffled tank, it is necessary to model the flow as a sliding

mesh simulation.

.... Node Based Averaging of Particle Data

In general, the presence of DPM parcels may affect the continuous phase fluid flow meaning that

discrete phase source terms and particle data such as fluid drag, temperature, volume fraction, and

velocity can be integrated into the flow solver. By default in ANSYS Fluent, the effects of a particular

DPM parcel are applied only to the cells that intersect with the trajectory of that parcel. As an altern-

ative, Enable Node Based Averaging is offered which distributes the effects of a DPM parcel even

into neighboring cells that share at least a mesh node with the cells intersected by the trajectory.

This allows a reduction of grid dependency of DPM simulations, since each parcel’s effects on the

flow solver are distributed more smoothly across neighboring cells.

You can select Enable Node Based Averaging in the Numerics tab of the Discrete Phase Model

dialog box, as shown in Figure . : The Discrete Phase Model Dialog Box and the Numerics (p. ).

For non-DDPM cases, the Enable Node Based Averaging option is not available when the Linearize

Source Terms is selected.

When enabled, the node based averaging is applied to particle velocity, particle temperature, particle

volume fraction, and DPM concentration. By default, Average DPM Source Terms is also enabled,

which applies node averaging to the source terms as well. When the Dense Discrete Phase Model is

being used, the Average DDPM Variables option appears to provide node based averaging for the

discrete phase specific variables, such as DDPM particle drag. When Contour Plots for DPM Variables

is enabled (Reporting of Discrete Phase Variables (p. )), these quantities will also be node averaged.

Average in Each Integration Step should be enabled if you find that the flux report is showing dis-

crepancies for mass flow rates of particles injected into and leaving the domain. This option increases

computation time so it is not enabled by default.

Once you have selected Enable Node Based Averaging, you must also select the Averaging Kernel

to accumulate the particle related data on the mesh nodes and to redistribute them back to the finite

volume cells. The kernel and related settings are specified in the Kernel Settings section of the Dis-

crete Phase Model dialog box. The following kernels are available:

nodes-per-cell

shortest-distance

inverse-distance

gaussian

If you use the gaussian kernel, you must also specify the Gaussian Factor, which determines

the width of the Gaussian distribution. The default value is .

For details about the averaging and kernel equations, refer to Node Based Averaging in the Theory

Guide.

.... Linearized Source Terms

Source terms for discrete phase momentum, energy, and species can be linearized with respect to

the cell variable,

:

(.)

This linearization strongly increases numerical stability for steady flows. For transient flows, it typically

allows the use of larger time steps and larger under-relaxation factors for the DPM model.

You can enable source term linearization with the Linearize Source Terms option in the Numerics

tab of the Discrete Phase Model dialog box. For non-DDPM cases, the Linearize Source Terms option

is not available when the Enable Node Based Averaging is selected.

The source term linearization can be combined with the Update DPM Sources Every Flow Iteration

option (Options for Interaction with the Continuous Phase (p. )).

.... Staggering of Particles in Space and Time

In order to obtain a better representation of an injector, the particles can be staggered spatially and/or

temporally. When particles are staggered spatially, ANSYS Fluent randomly samples from the region

in which the spray is specified (for example, the sheet thickness in the pressure-swirl atomizer) so

that as the calculation progresses, trajectories will originate from the entire region. This allows the

entire geometry specified in the atomizer to be sampled while specifying fewer streams in the input

dialog box, thus decreasing computational expense.

You can enable injection-specific spatial staggering of the particles by selecting the Stagger Positions

option in the Stagger Options group box in the Point Properties tab of the Set Injection Properties

dialog box and then, if applicable, specifying Stagger Radius to define the region from which particles

are released. For more information, see the appropriate sections for injection-specific point properties.

You can also enable injection-specific spatial staggering of the particles by issuing the following text

commands:

/define/models/dpm/options/stagger-spatially-atomizer-injections?

/define/models/dpm/options/stagger-spatially-standard-injections?

When spatial staggering is enabled for non-atomizer injections, a stagger radius must be specified

by using the text command:

/define/models/dpm/options/stagger-radius

When injecting particles in a transient calculation using relatively large time steps in relation to the

spray event, the particles can clump together in discrete bunches. The clumps do not look physically

realistic, though ANSYS Fluent calculates the trajectory for each particle as it passes through a cell

and the coupling to the gas phase is properly accounted for. To obtain a statistically smoother rep-

resentation of the spray, the particles can be staggered in time. During the first time step, the particle

is tracked for a random percentage of its initial step. This results in a sample of the initial volume

swept out by the particle during the first time step and a smoother, more uniform spatial distribution

at longer time intervals.

The following setup commands for staggering in time are available in the text user interface (TUI):

stagger-temporally?

staggering-factor

The “staggering factor” is applied to temporal staggering only. It is a constant that multiplies the time

step size to give the random sampling interval. The staggering factor controls the percentage of every

particle’s initial time step that will be sampled. For example, if the staggering factor is ., then the

parcels in the injection will be tracked between half and all of their full initial time step. If the stag-

gering factor is ., then the parcels will be tracked between ninety percent and all of their initial

time step. If the staggering factor is set to ., the parcels will be tracked between ten percent and

all of their initial time step. This allows you to control the amount of smoothing between injections.

The default values for the options in the TUI are spatial staggering for atomizers (including the solid-

cone), no temporal staggering and a temporal staggering factor of .. The temporal staggering factor

is inactive until the flag for temporal staggering is enabled.

.... Under-Relaxing Lagrangian Wall Film Height

As the wall film moves and spreads on the wall faces, under-relaxation is applied to the film height

computation. The under-relaxation factor can be specified using the following text command:

define/models/dpm/numerics/underrelax-film-height

A lower under-relaxation factor results in a smoother film appearance, especially closer to the film

edge. However, it may distort the film shape, especially for cases where high velocity droplets are

impinging on the film. The recommended values range between . (default) and ..

The primary inputs that you must provide for the discrete phase calculations in ANSYS Fluent are the

initial conditions that define the starting positions, velocities, and other parameters for each particle

stream and the physical effects acting on the particle streams, requiring additional particle properties.

You will define the initial conditions for a particle/droplet stream by creating an “injection” and assigning

properties to it.

The required initial conditions depend on the injection type, while the physical effects are selected by

choosing an appropriate particle type. For some injection types you can provide a particle size distribu-

tion, like the Rosin-Rammler distribution, see Using the Rosin-Rammler Diameter Distribution Meth-

od (p. ).

The initial conditions provide the starting values for all of the dependent discrete phase variables that

describe the instantaneous conditions of an individual particle, and include the following:

,  coordinates) of the particle

velocities ( , ,

) of the particle

Velocity magnitudes and spray cone angle can also be used (in 3D) to define the initial velocities (see

Point Properties for Cone Injections (p. )). For moving reference frames, relative velocities should

be specified.

diameter of the particle,

temperature of the particle,

Setting Initial Conditions for the Discrete Phase

mass flow rate of the particle stream that will follow the trajectory of the individual particle/droplet,

(required only for coupled calculations)

additional parameters if one of the atomizer models described in Atomizer Model Theory in the Theory

Guide is used for the injection

Important

When an atomizer model is selected, you will not specify initial diameter, velocity, and

position quantities for the particles due to the complexities of sheet and ligament breakup.

Instead of initial conditions, the quantities you will specify for the atomizer models are

global parameters.

These dependent variables (temperature, diameter, and so on) are updated according to the equations

of motion (Particle Motion Theory in the Theory Guide) and according to the heat/mass transfer relations

applied (Laws for Heat and Mass Exchange in the Theory Guide) as the particle/droplet moves along

its trajectory. You can define any number of different sets of initial conditions for discrete phase

particles/droplets provided that your computer has sufficient memory.

For the setup of transient particle cases, the point properties for mass flow and velocity can be specified

using transient profiles (see Point Properties for Transient Injections (p. )).

... Injection Types

... Particle Types

... Point Properties for Single Injections

... Point Properties for Group Injections

... Point Properties for Cone Injections

... Point Properties for Surface Injections

... Point Properties for Plain-Orifice Atomizer Injections

... Point Properties for Pressure-Swirl Atomizer Injections

... Point Properties for Air-Blast/Air-Assist Atomizer Injections

... Point Properties for Flat-Fan Atomizer Injections

... Point Properties for Effervescent Atomizer Injections

... Point Properties for File Injections

... Point Properties for Condensate Injections

... Using the Rosin-Rammler Diameter Distribution Method

... Creating and Modifying Injections

... Defining Injection Properties

... Specifying Injection-Specific Physical Models

... Specifying Turbulent Dispersion of Particles

... Custom Particle Laws

... Defining Properties Common to More than One Injection

... Point Properties for Transient Injections

ANSYS Fluent provides  types of injections:

single

group

cone (only in 3D)

surface

plain-orifice atomizer

pressure-swirl atomizer

air-blast-atomizer

flat-fan-atomizer

effervescent-atomizer

file

condensate

For each nonatomizer injection type, you will specify each of the initial conditions listed in Setting

Initial Conditions for the Discrete Phase (p. ), the type of particle that possesses these initial conditions,

and any other relevant parameters for the particle type chosen.

When defining injection point properties for the following injection types:

single

group

all cone injections

all atomizer injections

you can interactively preview the current injection position and orientation in the graphics window

prior to saving the settings. When you click Update Injection Display in the Set Injection Properties

dialog box or Set Multiple Injection Properties dialog box, ANSYS Fluent will apply the current settings

to the injection display. Once you click OK in the Set Injection Properties dialog box or Apply in the

Set Multiple Injection Properties dialog box, the injection properties will be saved, and the graphics

window will be once more updated. When you open the Set Injection Properties dialog box for the

existing injection, ANSYS Fluent will also automatically display the injection in the graphics window.

The injection position and orientation will not be displayed if you use profiles to specify the injection

position and direction. If you use the DEFINE_DPM_INJECTION_INIT user-defined function, the

displayed injection position and orientation will reflect only the default point properties for the specific

injection type.

You should create a single injection when you want to specify a single value for each of the initial

conditions (Figure . : Particle Injection Defining a Single Particle Stream (p. )). Create a group in-

jection (Figure . : Particle Injection Defining an Initial Spatial Distribution of the Particle

Streams (p. )) when you want to define a range for one or more of the initial conditions (for example,

a range of diameters or a range of initial positions). To define cone injections in 3D problems, create

a cone injection and specify a particle release pattern (point, hollow, ring, or solid) (Figure . : Particle

Injection Defining an Initial Spray Distribution of the Particle Velocity (p. )). To release particles from

a surface (either a zone surface or a surface you have defined using Create in the Domain ribbon tab

(Surfacegroup box)), you will create a surface injection. (If you create a surface injection, a particle

stream will be released from each facet of the surface. You can use the Bounded and Sample Points

options in the Plane Surface dialog box to create injections from a rectangular mesh of particles in

3D (see Plane Surfaces (p. ) for details). If you are modeling film condensation, use the condensate

injection type to define the vapor-liquid material pair and other modeling settings for the film con-

densation process.

Figure . : Particle Injection Defining a Single Particle Stream

Figure . : Particle Injection Defining an Initial Spatial Distribution of the Particle Streams

Figure . : Particle Injection Defining an Initial Spray Distribution of the Particle Velocity

Particle initial conditions (position, velocity, diameter, temperature, and mass flow rate) can also be

read from an external file if none of the injection types listed above can be used to describe your in-

jection distribution.

The inputs for setting injections are described in detail in Defining Injection Properties (p. ).

When you define a set of initial conditions (as described in Defining Injection Properties (p. )), you

will need to specify the type of particle. The particle types available to you depend on the range of

physical models that you have defined.

A massless particle is a discrete element that follows the flow and temperature of the continuous phase.

As it has no mass, it has no associated physical properties, and no force is exerted on it. However, you can

assign a User-Defined Law to be applied to the massless particle.The massless particle type is available

with all ANSYS Fluent models.

An inert particle is a discrete phase element (particle, droplet, or bubble) that obeys the force balance

(Equation . in the Theory Guide) and is subject to heating or cooling via Law  (Inert Heating or Cooling

(Law /Law ) in the Theory Guide).The inert type is available for all ANSYS Fluent models.

A droplet particle is a liquid droplet in a continuous-phase gas flow that obeys the force balance (Equa-

tion . in the Theory Guide) and that experiences heating/cooling via Law  followed by vaporization

and boiling via Laws  and  (Droplet Vaporization (Law ) and Droplet Boiling (Law ) in the Theory Guide).

The droplet type is available when heat transfer is being modeled and at least two chemical species are

active or the non-premixed or partially premixed combustion model is active.You should use the ideal gas

law to define the gas-phase density (in the Create/Edit Materials dialog box, as discussed in Density Inputs

for the Incompressible Ideal Gas Law (p. )) when you select the droplet type.

A combusting particle is a solid particle that obeys the force balance (Equation . ), and, after an initial

phase of inert heating (Law ), undergoes devolatization (Devolatilization (Law )) and then a heterogeneous

surface reaction via Law  (Surface Combustion (Law ) in the Theory Guide). Finally, the nonvolatile portion

of a combusting particle is subject to inert heating via Law .You can also include an evaporating material

with the combusting particle by selecting the Wet Combustion option in the Set Injection Properties

Dialog Box (p. ).This allows you to include a material that evaporates and boils via Laws  and  (Droplet

Vaporization (Law ) and Droplet Boiling (Law ) in the Theory Guide) before devolatilization of the particle

material begins.The combusting type is available when heat transfer is being modeled and at least three

chemical species are active or the non-premixed combustion model is active.You should use the ideal gas

law to define the gas-phase density (in the Create/Edit Materials Dialog Box (p. )) when you select the

combusting particle type.

A multicomponent particle is, as the name implies, a droplet particle containing a mixture of several

components or species.The conservation equations of all components, the energy equation, and vapor-

liquid-equilibrium at the multicomponent particle surface form a coupled system of differential equations.

Law , the multicomponent law (Multicomponent Particle Definition (Law ) in the Theory Guide) is used

for such systems.You should use the volume weighted mixing law to define the particle mixture density

(in the Create/Edit Materials Dialog Box (p. )) when you select the particle-mixture material type.

Laws

Activated

Particle Type

–

–

Massless

,

inert/heating or cooling

Inert

, , ,

heating/evaporation/boiling

Droplet

, , ,

heating; evolution of volatiles/swelling; heterogeneous surface reaction

Combusting

multicomponent droplets/particles

Multicomponent

For a single injection, you will define the following initial conditions for the particle stream under the

Point Properties heading (in the Set Injection Properties Dialog Box (p. )):

position

Set the ,

, and  positions of the injected stream along the Cartesian axes of the problem geometry

in the X-, Y-, and Z-Position fields. (Z-Position will appear only for 3D problems.)

velocity

Set the ,

, and  components of the stream’s initial velocity in the X-, Y-, and Z-Velocity fields.

(Z-Velocity will appear only for 3D problems.)

angular velocity (available when particle rotation is enabled (see Particle Rotation (p. )))

Set the ,

, and  components of the stream’s initial velocity in the X-, Y-, and Z-Angular-Velocity

fields. (Only Z-Angular-Velocity will appear for 2D problems, because rotation in 2D occurs in the

plane, that is, the rotation vector is normal to the plane.)

diameter

Set the initial diameter of the injected particle stream in the Diameter field.

Set the initial (absolute) temperature of the injected particle stream in the Temperature field.

mass flow rate

For coupled phase calculations (see Solution Strategies for the Discrete Phase (p. )), set the mass

of particles per unit time that follows the trajectory defined by the injection in the Flow Rate field.

Note that in axisymmetric problems the mass flow rate is defined per

radians and in 2D problems

per unit meter depth (regardless of the reference value for length).

duration of injection

For unsteady particle tracking (see Steady/Transient Treatment of Particles (p. )), set the starting

and ending time for the injection in the Start Time and Stop Time fields. When In-Cylinder mesh

motion is enabled, set the starting and ending crank angles for the injection in the Start Crank

Angle and Stop Crank Angle fields. The values you enter are for one complete engine cycle. In

subsequent cycles, the injection will be started and stopped according to Equation . (p. ),

where

corresponds to the injection start or end crank angle.

For the massless particle type, you will only need to define the position of the injection. The particle

injection velocity is set by the solver equal to the velocity of the continuous phase at the injection

point.

If you want to randomly distribute the initial placement of the particles, you can enable Stagger Pos-

itions and specify Stagger Radius to define the particle release region. For more information on

spatial staggering, see Staggering of Particles in Space and Time (p. ). This option is disabled by

default.

For group injections, you will define the properties position, velocity, angular velocity (available when

default.

particle rotation is enabled (see Particle Rotation (p. ))), diameter, temperature, and flow rate for

the First Point and Last Point in the group. That is, you will define a range of values,

through

,

for each initial condition

by setting values for

and

. ANSYS Fluent assigns a value of

to the

th injection in the group using a linear variation between the first and last values for

:

(.)

Thus, for example, if your group consists of  particle streams and you define a range for the initial

location from . to . meters, the initial  location of each stream is as follows:

Stream :  = . meters

Important

In general, you should supply a range for only one of the initial conditions in a given

group—leaving all other conditions fixed while a single condition varies among the stream

numbers of the group. Otherwise you may find, for example, that your simultaneous inputs

of a spatial distribution and a size distribution have placed the small droplets at the begin-

ning of the spatial range and the large droplets at the end of the spatial range.

The specified flow rate is defined per particle stream and can also be interpolated using Equa-

tion . (p. ). When a Rosin-Rammler sized distribution is specified the total flow rate will be specified.

For the massless particle type, you will only need to define the first and last point of the injection

group position. The particle velocities are set by the solver equal to the velocity of the continuous

phase at the injection points.

Note that you can use a different method for defining the size distribution of the particles, as discussed

below.

To randomly distribute the initial placement of the particles, enable Stagger Positions and specify

Stagger Radius to define the particle release region. For more information on spatial staggering, see

Staggering of Particles in Space and Time (p. ). This option is disabled by default.

In 3D problems, you can define the following types of particle stream cones:

point-cone

hollow-cone

ring-cone

solid-cone

The particles are released from a 2D region that may be a point, a circle, or an annulus. Its geometry,

location, and orientation as well as the shape of the spray cone are defined by the injection parameters.

Once you select a cone injection type from the Cone Type drop-down list, (the Cone Injector Para-

meters group box in the Point Properties tab of the Set Injection Properties dialog box), the para-

meters specific to the selected injection type will be displayed. These inputs are summarized below.

Refer to Figure . : Cone Injector Geometry (p. ) for an illustration of the geometry.

Figure . : Cone Injector Geometry

position

Set the coordinates of the origin of the spray cone in the X-, Y-, and Z-Position fields (  in Fig-

ure . : Cone Injector Geometry (p. ))

diameter

Set the diameter of the particles in the stream in the Diameter field.

Set the temperature of the streams in the Temperature field.

diameter

Angle and Stop Crank Angle fields.

axis

Set the ,

, and  components of the vector defining the cone’s axis in the X-Axis, Y-Axis, and Z-

Axis fields. (  in Figure . : Cone Injector Geometry (p. ))

velocity

Set the velocity magnitude of the particle streams that will be oriented along the specified spray

cone in the Velocity Magnitude field. (

in Figure . : Cone Injector Geometry (p. ))

Note

This is the total spray velocity magnitude and includes any swirl component in a hollow

cone injector.

angular velocity

Set the angular velocity magnitude of the particle streams that will be oriented along the specified

spray cone in the Angular Velocity Magnitude field.

cone angle

Set the included half-angle of the spray cone in the Cone Angle field. (  in Figure . : Cone In-

jector Geometry (p. ))

radii

For hollow-cone, ring-cone, and solid-cone injections, specify the Outer Radius.

For ring-cone injections, specify a nonzero Inner Radius to model injectors that do not emanate

from a single point. The particles will be distributed about the axis with the specified radius. (  in

Figure . : Cone Injector Geometry (p. ))

swirl fraction (hollow cone only)

Set the swirl fraction, which determines the relative magnitude of the swirl velocity, in the Swirl

Fraction field.

The direction of the swirl component is defined using the right-hand rule about the cone axis (a

negative value for the swirl fraction can be used to reverse the swirl direction).

For coupled calculations, set the total mass flow rate for the streams in the spray cone in the Total

Flow Rate field. Note that for a 3D sector, the flow rate must be appropriate for the sector defined

by the Azimuthal Start Angle and Azimuthal Stop Angle.

azimuthal angles

For 3D sectors, set the Azimuthal Start Angle and Azimuthal Stop Angle to define the sector. (

and , respectively, in Figure . : Cone Injector Geometry (p. )).

The Azimuthal Start Angle and Azimuthal Stop Angle are specified with respect to a reference

vector,

, that is orthogonal to both the cone axis and the global X axis. The reference vector,

,

can be determined as the cross product of the cone axis and the global X axis.

where  is a unit vector along the global X axis. In the case that the cone axis is along the X axis,

then  is along the Y axis.

In addition to the above parameters, you can select the following options:

Uniform Massflow Distribution (solid-cone or ring-cone): Specifies a uniform spacial distribution of mass

over the cross-section of a cone.This is especially important when the mesh cell size is smaller than the

particle diameter or another characteristic size.This option is enabled by default.

Stagger Positions: Specifies a random spatial distribution of particle steams. For hollow-cone injections

you must also specify Stagger Radius to define the region over which particle release points are staggered

in space. For more information on spatial staggering, see Staggering of Particles in Space and Time (p. ).

The distribution of the velocity directions in the particle streams for the point-cone, ring-cone, and

solid-cone injections is random. Furthermore, duplicating this injection may not necessarily result in

the same distribution, at the same location.

Important

For transient calculations, the spatial distribution of streams at the initial injection location

is recalculated at each time step. Sampling different possible trajectories allows a more ac-

curate representation of a point, ring, or solid cone using fewer computational parcels. For

steady-state calculations, the trajectories are initialized one time and kept the same for

subsequent DPM iterations. The trajectories are recalculated when a change in the Injections

dialog box occurs or when a case and data file are saved. If the residuals and solution change

when a small change is made to the injection or when a case and data file are saved, it may

mean that there are not enough trajectories being used to represent the point, ring, or

solid cone with sufficient accuracy.

Note that you may want to define multiple spray cones emanating from the same initial location in

order to specify a known size distribution of the spray or to include a known range of cone angles.

For the massless particle type, you will only need to define position, axis, cone angle, azimuthal angles,

and radius. The particle velocities are set by the solver equal to the velocity of the continuous phase

at the injection points.

For surface injections, you will define all the properties described in Point Properties for Single Injec-

tions (p. ) for single injections except for the initial position of the particle streams. The initial positions

of the particles will be the location of the data points on the specified surface(s). Note that you will

set the Total Flow Rate of all particles released from the surface (required for coupled calculations

only). If you want, you can scale the individual mass flow rates of the particles by the ratio of the area

of the face they are released from to the total area of the surface. To scale the mass flow rates, select

the Scale Flow Rate By Face Area option under Point Properties. For the massless particle type, you

will not need to enter any information to define a surface injection. The particle velocities are set by

the solver equal to the velocities of the continuous phase at the injection points.

Note that many surfaces have nonuniform distributions of points. If you want to generate a uniform

spatial distribution of particle streams released from a surface in 3D, you can create a bounded plane

surface with a uniform distribution using the Plane Surface Dialog Box (p. ), as described in Plane

Surfaces (p. ). In 2D, you can create a rake using the Line/Rake Surface Dialog Box (p. ), as described

in Line and Rake Surfaces (p. ).

In addition to the option of scaling the flow rate by the face area, the normal direction of a face can

be used for the injection direction. To use the face normal direction for the injection direction, select

the Inject Using Face Normal Direction option under Point Properties (Figure . : Setting Surface

Injection Properties (p. )). Once this option is selected, you only need to specify the velocity magnitude

of the injection, not the individual components of the velocity magnitude.

Important

Only surface injections from boundary surfaces will be moved with the mesh when a sliding

mesh or a moving or deforming mesh is being used.

For moving or deforming mesh simulations, only zonal surfaces can be selected.

A nonuniform size distribution can be used for surface injections, as described below.

.... Using the Rosin-Rammler Diameter Distribution Method

The Rosin-Rammler size distributions described in Using the Rosin-Rammler Diameter Distribution

Method (p. ) for group injections is also available for surface injections. If you select one of the

Rosin-Rammler distributions (rosin-rammler or rosin-rammler-logarithmic), you will need to specify

the following parameters under Point Properties, in addition to the initial velocity, temperature, and

total flow rate:

Min. Diameter

This is the smallest diameter to be considered in the size distribution.

Max. Diameter

This is the largest diameter to be considered in the size distribution.

Mean Diameter

This is the size parameter,

, in the Rosin-Rammler equation (Equation . (p. )).

Spread Parameter

This is the exponential parameter,

, in Equation . (p. ).

Number of Diameters

This is the number of diameters in each distribution (that is, the number of different diameters in

the stream injected from each face of the surface).

ANSYS Fluent will inject streams of particles from each face on the surface, with diameters defined

by the Rosin-Rammler distribution function. The total number of injection streams tracked for the

surface injection will be equal to the number of diameters in each distribution (Number of Diameters)

multiplied by the number of faces on the surface.

For a plain-orifice atomizer injection, you will define the following initial conditions under Point

Properties:

position

Set the ,

in the X-Position, Y-Position, and Z-Position fields. (Z-Position will appear only for 3D problems).

axis (3D only)

Set the ,

, and  components of the vector defining the axis of the orifice in the X-Axis, Y-Axis,

and Z-Axis fields.

Set the total mass flow rate for the streams in the atomizer in the Flow Rate field. Note that in 3D

sectors, the flow rate must be appropriate for the sector defined by the Azimuthal Start Angle and

Azimuthal Stop Angle.

vapor pressure

Set the vapor pressure governing the flow through the internal orifice (

in Table . : List of Gov-

erning Parameters for Internal Nozzle Flow in the Theory Guide) in the Vapor Pressure field.

diameter

Set the diameter of the orifice in the Injector Inner Diameter field (  in Table . : List of Governing

Parameters for Internal Nozzle Flow in the Theory Guide).

orifice length

Set the length of the orifice in the Orifice Length field (  in Table . : List of Governing Parameters

for Internal Nozzle Flow in the Theory Guide).

radius of curvature

Set the radius of curvature of the inlet corner in the Corner Radius of Curvature field (  in

Table . : List of Governing Parameters for Internal Nozzle Flow in the Theory Guide).

nozzle parameter

Set the constant for the spray angle correlation in the Constant A field (

the Theory Guide).

For 3D sectors, set the Azimuthal Start Angle and Azimuthal Stop Angle.

See The Plain-Orifice Atomizer Model in the Theory Guide for details about how these inputs are used.

If you want to randomly distribute the initial placement of the particles, enable Stagger Positions

(default). The region over which particle release points will be staggered is defined by the specified

orifice diameter. For more information on spatial staggering, see Staggering of Particles in Space and

Time (p. ).

For a pressure-swirl atomizer injection, you will specify some of the same properties as for a plain-orifice

atomizer. In addition to the position, axis (if 3D), temperature, mass flow rate, duration of injection (if

unsteady), injector inner diameter, and azimuthal angles (if relevant) described in Point Properties for

Plain-Orifice Atomizer Injections (p. ), you will need to specify the following parameters under Point

spray angle

Set the value of the spray angle of the injected stream in the Spray Half Angle field (  in Equa-

pressure

Set the absolute pressure upstream of the injection in the Upstream Pressure field (

in

sheet breakup

Set the value of the empirical constant that determines the length of the ligaments that are formed

after sheet breakup in the Sheet Constant field (

ligament diameter

For short waves, set the proportionality constant that linearly relates the ligament diameter,

, to

the wavelength that breaks up the sheet in the Ligament Constant field (see Equation .—Equa-

dispersion angle

For a smooth distribution of the droplets, the initial velocities is varied within this dispersion angle.

A sketch of the Atomizer Dispersion Angle for a flat fan atomizer is depicted in Figure . : Flat

Fan Viewed from Above and from the Side (p. ).

See The Pressure-Swirl Atomizer Model in the Theory Guide for details about how these inputs are

used.

For an air-blast/air-assist atomizer, you will specify some of the same properties as for a plain-orifice

outer diameter

Set the outer diameter of the injector in the Injector Outer Diameter field. This value is used in

conjunction with the Injector Inner Diameter to set the thickness of the liquid sheet (  in Equa-

Set the initial trajectory of the film as it leaves the end of the orifice in the Spray Half Angle field

(  in Equation . in the Theory Guide).

relative velocity

Set the maximum relative velocity that is produced by the sheet and air in the Relative Velocity

field.

For short waves, set the proportionality constant (

in Equation . in the Theory Guide) that

linearly relates the ligament diameter,

, to the wavelength that breaks up the sheet in the Ligament

Constant field.

See The Air-Blast/Air-Assist Atomizer Model in the Theory Guide for details about how these inputs are

used.

The flat-fan atomizer model is available only for 3D models. For this type of injection, you will define

the following initial conditions under Point Properties:

arc position

Set the coordinates of the center point of the arc from which the fan originates in the X-Center, Y-

Center, and Z-Center fields (see Figure . : Flat Fan Viewed from Above and from the Side (p. )).

virtual position

Set the coordinates of the virtual origin of the fan in the X-Virtual Origin, Y-Virtual Origin, and Z-

Virtual Origin fields. This point is the intersection of the lines that mark the sides of the fan (see

Figure . : Flat Fan Viewed from Above and from the Side (p. )).

normal vector

Set the direction that is normal to the fan in the X-Fan Normal Vector, Y-Fan Normal Vector, and

Z-Fan Normal Vector fields.

Set the mass flow rate for the streams in the atomizer in the Flow Rate field.

spray half angle

Set the initial half angle of the drops as they leave the end of the orifice in the Spray Half Angle

field.

orifice width

Set the width of the orifice (in the normal direction) in the Orifice Width field.

after sheet breakup in the Flat Fan Sheet Constant field (see Equation . in the Theory Guide).

A sketch of the Atomizer Dispersion Angle is depicted in Figure . : Flat Fan Viewed from Above

and from the Side (p. ).

See The Flat-Fan Atomizer Model in the Theory Guide for details about how these inputs are used.

To randomly distribute the initial placement of the particles, enable Stagger Positions (default). The

orifice width is used as radius to define the region over which particle release points will be staggered

in space. For more information on spatial staggering, see Staggering of Particles in Space and

Time (p. ).

Figure . : Flat Fan Viewed from Above and from the Side

Time (p. ).

For an effervescent atomizer injection, you will specify some of the same properties as for a plain-orifice

atomizer. In addition to the position, axis (if 3D), temperature, mass flow rate (including both flashing

and non-flashing components), duration of injection (if unsteady), vapor pressure, injector inner dia-

meter, and azimuthal angles (if relevant) described in Point Properties for Plain-Orifice Atomizer Injec-

tions (p. ), you will need to specify the following parameters under Point Properties:

mixture quality

Set the mass fraction of the injected mixture that vaporizes in the Mixture Quality field (  in

Equation . in the Theory Guide).

saturation temperature

Set the saturation temperature of the volatile substance in the Saturation Temp. field.

droplet dispersion

Set the parameter that controls the spatial dispersion of the droplet sizes in the Dispersion Constant

field (

Set the initial trajectory of the film as it leaves the end of the orifice in the Maximum Half Angle

field.

See The Effervescent Atomizer Model in the Theory Guide for details about how these inputs are used.

File injections can operate in two different modes, depending on the format of the file:

A steady file can be used in both steady and unsteady particle tracking. In the former case, for every line

entry in the file, a new particle parcel is generated for every injection time step in the usual way. By default,

injection time steps are identical to the global fluid-flow time steps; however, you can change it in the

Discrete Phase Model dialog box.

An unsteady file can only be used in unsteady particle tracking. Here, every line entry in the file contains

a time stamp (flow-time in the 13th column). At the appropriate simulated flow-time, ANSYS Fluent

will inject a single particle parcel only once.That means that during the entire time interval that it spans,

an unsteady injection file produces as many particle parcels as the number of the data line entries in the

file.

An unsteady file can be converted into a steady-state injection file as described in Data Reduction of

Samples (p. ).

The injection file mode is determined by the file header:

If the file does not have any header, then it is treated as a steady file for backward compatibility reasons.

If the file contains a header of the expected format, the information in the header will determine whether

the file operates in the steady or unsteady mode as further described.

Important

Using an unsteady injection file for steady particle tracking will result in an error.

.... Steady File Format

The steady file for a file injection has the following form:

(( x y z u v w diameter temperature mass-flow) name )

with all of the words denoting numeric parameters in scientific floating-point notation in SI units. All

the parentheses are required, but the name is optional.

Sample files generated during sampling of trajectories for steady particle tracking as described in

Sampling of Trajectories (p. ) can also be used as steady injection files since they have a similar

The file can have an optional two-line header automatically generated by particle sampling for steady

particle tracking in the following form:

(z= )

( x  y  z  u  v  w  diameter  t  mass-flow  mass  frequency  time  name)

In the first line, you can replace z= with an arbitrary label that must not contain any white-space

characters. You must not change the rest of the header, but you can add any number of white space

characters between its elements.

.... Unsteady File Format

The unsteady file must have a two-line header of the following format:

(z= )

( x  y  z  u  v  w  diameter  t  parcel-mass  mass  n-in-parcel  time  flow-time  name)

characters between its elements. The header is automatically written by ANSYS Fluent into every

sampling file for unsteady particle tracking.

The unsteady file for a file injection has the following form:

(( x  y  z  u  v  w  diameter  temperature  parcel-mass  mass  n-in-parcel  time  flow-time)  name)

Like for the steady file format, all the numbers must be in SI units, and all the parentheses are required,

but the name is optional. A file that ANSYS Fluent writes from unsteady particle tracking can be used

as an injection file in the unsteady mode.

An unsteady injection file can contain additional columns that can be processed using a

DEFINE_DPM_INJECTION_INIT UDF. For details, see DEFINE_DPM_INJECTION_INIT in the

Note

Note

In an unsteady injection file, all entries must be sorted strictly in ascending order of the

simulated flow-time (13th column). If you use unsteady particle sampling in ANSYS

Fluent to generate such a file, you must select the Sort Sample Files option in the Sample

Trajectories dialog box.

.... User Input for File Injections

In the Point Properties tab in the Set Injection Properties dialog box, you can specify the following

injection parameters:

Start Time

specifies the simulated time when ANSYS Fluent starts to inject particles from this injection.

Stop Time

specifies the simulated time when ANSYS Fluent stops to inject particles from this injection.

Start Flow-time in File

(optional) determines the line from which ANSYS Fluent starts reading the injection file. All line entries

in which flow-time (13th column) is less than the specified value will be skipped. For remaining lines,

the injection release time is determined as:

Start Time + flow-time - Start Flow-time in File

The default value of  means that ANSYS Fluent will read the injection file starting from the first

line entry.

Repeat Interval in File

(optional) can be used to put the unsteady injection into a time-periodic mode. Once ANSYS Fluent has

read the injection file for the specified time period, it rewinds the file and starts reading it again from

the line from which it began.This cycling process continues until Stop Time is reached. In this way, de-

tailed data for a small time interval can be used to approximate a steady state over longer time periods

in an unsteady simulation with unsteady particle tracking.The default value of  means no repetition

in time.

in time.

Note

For steady injection files, Start Flow-time in File and Repeat Interval in File are ignored.

For a condensate injection, you will define only the duration of the injection by setting the starting

and ending time for the injection in the Start Time and Stop Time fields under the Point Properties

tab in the Set Injection Properties dialog box. The duration of the injection determines the time

during which film condensation will be initiated on the walls that have the Film Condensation option

enabled.

For liquid sprays, a convenient representation of the droplet size distribution is the Rosin-Rammler

expression. The complete range of sizes is divided into an adequate number of discrete intervals; each

represented by a mean diameter for which trajectory calculations are performed. If the size distribution

is of the Rosin-Rammler type, the mass fraction of droplets of diameter greater than  is given by

(.)

where  is the size constant and  is the size distribution parameter.

By default, you will define the size distribution of particles by inputting a diameter for the first and

last points and using the linear equation (Equation . (p. )) to vary the diameter of each particle

stream in the group. When you want a different mass flow rate for each particle/droplet size, however,

the linear variation may not yield the distribution you need. Your particle size distribution may be

defined most easily by fitting the size distribution data to the Rosin-Rammler equation. In this approach,

the complete range of particle sizes is divided into a set of discrete size ranges, each to be defined by

a single stream that is part of the group. Assume, for example, that the particle size data obeys the

following distribution:

Mass Fraction in Range

Diameter Range ( m)

.

–

.

–

.

–

.

–

.

–

.

–

The Rosin-Rammler distribution function is based on the assumption that an exponential relationship

exists between the droplet diameter,

, and the mass fraction of droplets with diameter greater than

,

:

(.)

ANSYS Fluent refers to the quantity  in Equation . (p. ) as the Mean Diameter and to  as the

Spread Parameter. These parameters are specified by you (in the Set Injection Properties Dialog

Box (p. ) under the First Point heading) to define the Rosin-Rammler size distribution. To solve for

these parameters, you must fit your particle size data to the Rosin-Rammler exponential equation. To

determine these inputs, first recast the given droplet size data in terms of the Rosin-Rammler format.

For the example data provided above, this yields the following pairs of  and

:

Mass Fraction with Diameter

Greater than ,

Diameter,

( m)

.

.

.

.

.

(.)

A plot of

vs.

is shown in Figure . : Example of Cumulative Size Distribution of Particles (p. ).

Figure . : Example of Cumulative Size Distribution of Particles

Next, derive values of  and  such that the data in Figure . : Example of Cumulative Size Distribution

of Particles (p. ) fit Equation . (p. ). The value for  is obtained by noting that this is the value

of  at which

. From Figure . : Example of Cumulative Size Distribution of

of  at which

Particles (p. ), you can estimate that this occurs for

m. The numerical value for  is given

by

(.)

By substituting the given data pairs for

and

into this equation, you can obtain values for

and find an average. Doing so yields an average value of  = . for the example data above. The

resulting Rosin-Rammler curve fit is compared to the example data in Figure . : Rosin-Rammler

Curve Fit for the Example Particle Size Data (p. ). You can enter values for  and , as well as the

diameter range of the data and the total mass flow rate for the combined individual size ranges, using

the Set Injection Properties Dialog Box (p. ).

This technique of fitting the Rosin-Rammler curve to spray data is used when reporting the Rosin-

Rammler diameter and spread parameter in the Discrete Phase Summary dialog box in Summary

Reporting of Current Particles (p. ).

Figure . : Rosin-Rammler Curve Fit for the Example Particle Size Data

A second Rosin-Rammler distribution is also available based on the natural logarithm of the particle

diameter. If in your case, the smaller-diameter particles in a Rosin-Rammler distribution have higher

mass flows in comparison with the larger-diameter particles, you may want better resolution of the

smaller-diameter particle streams, or “bins”. You can therefore choose to have the diameter increments

in the Rosin-Rammler distribution done uniformly by

.

In the standard Rosin-Rammler distribution, a particle injection may have a diameter range of  to

.

m. In the logarithmic Rosin-Rammler distribution, the same diameter range would be converted to

a range of

to

, or about  to .. In this way, the mass flow in one bin would be less-heavily

skewed as compared to the other bins.

When a Rosin-Rammler size distribution is being defined for the group of streams, you should define

(in addition to the initial velocity, position, and temperature) the following parameters, which appear

under the heading for the First Point:

Total Flow Rate

This is the total mass flow rate of the

streams in the group. Note that in axisymmetric problems

this mass flow rate is defined per

radians and in 2D problems per unit meter depth.

, in   Equation . (p. ).

....The Stochastic Rosin-Rammler Diameter Distribution Method

For atomizer injections, a Rosin-Rammler distribution is assumed for the particles exiting the injector.

In order to decrease the number of particles necessary to accurately describe the distribution, the

diameter distribution function is randomly sampled for each instance where new particles are intro-

duced into the domain.

The Rosin-Rammler distribution can be written as

(.)

where

is the mass fraction smaller than a given diameter

,

is the Rosin-Rammler diameter and

(.)

where

,

is the Rosin-Rammler exponent. This expression can be inverted by taking logs of both sides and

rearranging,

(.)

Given a mass fraction

along with parameters  and , this function will explicitly provide a diameter,

. Diameters for the atomizer injectors described in Point Properties for Plain-Orifice Atomizer Injec-

tions (p. ) are obtained by uniformly sampling

You will use the Injections branch in the Outline View and the Injections Dialog Box (p. ) (Fig-

ure . : The Injections Dialog Box (p. ), Figure . : The Injections Branch in the Outline View

(p. )) to create, copy, delete, list, read, and write injections.

New...

Figure . : The Injections Branch in the Outline View

Figure . : The Injections Dialog Box

(You can also click the Injections... button in the Discrete Phase Model Dialog Box (p. ) to open the

Injections dialog box.)

Note

[Linux Only] If you are not part of a video group, a session on a local Linux machine with

SLES11, SP4, and OpenGL may terminate abnormally during an injection setup for the discrete

phase model case. To avoid this issue, you should restart the ANSYS Fluent session with

the driver option -x11 or you should ensure that you are added to the video group on

that machine. Workaround: Deactivate the injection visualization during the case setup by

using the following scheme command:

rpsetvar 'dpm/visualize-injections? #f)

.... Creating Injections

To create an injection, click the Create button. The Set Injection Properties Dialog Box (p. ) will

open automatically to allow you to set the injection properties (as described in Defining Injection

Properties (p. )). After the injection is created, the new injection will appear in the Injections list,

.... Modifying Injections

To modify an existing injection, select its name in the Injections list and click the Set... button. The

Set Injection Properties dialog box will open, and you can modify the properties as needed.

If you have two or more injections for which you want to set some of the same properties, select

their names in the Injections list and click the Set... button. The Set Multiple Injection Properties

dialog box will open, which will allow you to set the common properties. For instructions about using

this dialog box, see Defining Properties Common to More than One Injection (p. ).

.... Copying Injections

To copy an existing injection to a new injection, select the existing injection in the Injections list and

click the Copy button. The Set Injection Properties Dialog Box (p. ) will open with a new injection

that has the same properties as the injection you selected. This is useful if you want to set another

injection with similar properties.

.... Deleting Injections

You can delete an injection by selecting its name in the Injections list and clicking the Delete button.

.... Listing Injections

To list the initial conditions for the particle streams in the selected injection, click the List button.

ANSYS Fluent reports the initial conditions (in SI units) in the console under various columns:

The particle stream number is in the column headed NO.

The particle type (IN for inert, DR for droplet, or CP for combusting particle) is in the column headed TYP.

The ,

, and  positions are in the columns headed (X), (Y), and (Z).

The ,

, and  velocities are in the columns headed (U), (V), and (W).

The temperature is in the column headed (T).

The diameter is in the column headed (DIAM).

The mass flow rate in the column headed (MFLOW).

.... Reading and Writing Injections

To transfer information about DPM injections from one case file to another, use the Read... and

Write... buttons. You can write selected injections to a file, which can be read into a different ANSYS

Fluent session, simplifying the setup of new case files. To write the injection, select the injection from

the list, then click Write.... The Select File Dialog Box (p. ) will open where you can enter the name

of your injection file. To read in an injection, click Read... to open The Select File Dialog Box (p. )

where you will select the injection file to read in. If the injection that you imported has the same

name as that in your current case, then ANSYS Fluent will rename the imported injection.

After reading injections, you may need to visit the Injections dialog box to modify the settings for

the injection material and the DPM laws since the presumed settings may have changed in the current

case file setup.

Once you have created an injection (using the Injections Dialog Box (p. ), as described in Creating

and Modifying Injections (p. )), you will use the Set Injection Properties Dialog Box (p. ) (Fig-

ure . : The Set Injection Properties Dialog Box (p. )) to define the injection properties. (Remember

that this dialog box will open when you create a new injection, or when you select an existing injection

and click the Set... button in the Injections dialog box.)

Figure . : The Set Injection Properties Dialog Box

The procedure for defining an injection is as follows:

. If you want to change the default name of the injection, enter a new name in the Injection Name field.

This is recommended if you are defining a large number of injections so you can easily distinguish them.

When assigning names to your injections, keep in mind the selection shortcut described in Creating and

Modifying Injections (p. ).

. Choose the type of injection in the Injection Type drop-down list.The injection choices (single, group,

cone, surface, plain-orifice-atomizer, pressure-swirl-atomizer, air-blast-atomizer, flat-fan-atomizer,

effervescent-atomizer, condensate, and file) are described in Injection Types (p. ). Note that if you

select any of the atomizer models, you also must set the Viscosity and Droplet Surface Tension in the

Important

Note that only surface injections from boundary surfaces will be moved with the mesh

when a sliding mesh or a moving or deforming mesh is being used.

Important

. If you are defining a single or condensate injection, go to the next step. For a group, cone, or any of the

atomizer injections, set the Number of Streams in the group, spray cone, or atomizer.

If you are defining a surface injection (see Figure . : Setting Surface Injection Properties (p. )),

choose the surface(s) from which the particles will be released in the Release From Surfaces list.

If you are reading the injection from a file, click the File... button at the bottom of the Set Injection

Properties Dialog Box (p. ) and specify the file to be read in the resulting Select File dialog box.

The parameters in the injection file must be in SI units.

Figure . : Setting Surface Injection Properties

. Select Massless, Inert, Droplet, Combusting, or Multicomponent as the Particle Type.The available

types are described in Particle Types (p. ). Note that for the condensate injection, the only available

particle types are Droplet and Multicomponent.

. Choose the material for the particle(s) in the Material drop-down list.

If this is the first time you have created a particle of this type, you can choose from all of the ma-

terials of this type defined in the database. If you have already created a particle of this type, the

only available material will be the material you selected for that particle. You can define additional

materials by copying them from the database or creating them from scratch, as discussed in Setting

Discrete-Phase Physical Properties (p. ) and described in detail in Using the Create/Edit Materials

Important

Note that you will not choose a Material for a Massless particle type.

. If you are defining a group, cone, or surface injection and you want to change from the default linear

(for group injections) or uniform (for cone and surface injections) interpolation method used to determine

the size of the particles, select rosin-rammler or rosin-rammler-logarithmic in the Diameter Distribution

drop-down list.The Rosin-Rammler method for determining the range of diameters for a group injection

is described in Using the Rosin-Rammler Diameter Distribution Method (p. ).

. If you have created a customized particle law using user-defined functions, enable the Custom option

under Laws and specify the appropriate laws as described in Custom Particle Laws (p. ).

. If your particle type is Inert, go to the next step. If you are defining Droplet particles, select the gas phase

species created by the vaporization and boiling laws (Laws  and ) in the Evaporating Species drop-

down list.

If you are defining Combusting particles, select the gas phase species created by the devolatilization

law (Law ) in the Devolatilizing Species drop-down list, the gas phase species that participates

in the surface char combustion reaction (Law ) in the Oxidizing Species list, and the gas phase

species created by the surface char combustion reaction (Law ) in the Product Species list. Note

that if the Combustion Model for the selected combusting particle material (in the Create/Edit

Materials dialog box) is the multiple-surface-reaction model, then the Oxidizing Species and

Product Species lists will be disabled because the reaction stoichiometry has been defined in the

mixture material.

If you are defining Multicomponent particles, maw  will go into effect. Notice that the Components

tab will become active when this particle type is selected. See below for information on the Com-

ponents tab.

. Click the Point Properties tab (the default), and specify the point properties (position, velocity, diameter,

temperature, and—if appropriate—mass flow rate and any atomizer-related parameters) as described for

each injection type in Point Properties for Single Injections (p. ) – Point Properties for Effervescent At-

omizer Injections (p. ).

For surface injections, you can enable the Scale Flow Rate by Face Area and you can choose the

injection direction. To use the face normal direction for the injection direction, select the Inject

Using Face Normal Direction option under Point Properties (Figure . : Setting Surface Injection

Properties (p. )). Once this option is selected, you only need to specify the velocity magnitude

. If you want to set up injection-specific physics models such as drag laws, Brownian motion, and breakup,

click the Physical Models tab and configure the injection physics models as described in Specifying Injec-

tion-Specific Physical Models (p. ).

. If the flow is turbulent and you want to include the effects of turbulence on the particle dispersion, click

the Turbulent Dispersion tab, enable the Discrete Random Walk Model under Stochastic tracking or

the Cloud Model, and set the related parameters as described in Specifying Turbulent Dispersion of

. If you have enabled Unsteady Particle Tracking, you can define settings for how the parcels are

released. Click the Parcel tab and select a Parcel Release Method from the drop-down list. The

default method is standard, in which a single parcel is released per injection stream per time step.

Alternatively can choose constant-number, constant-mass, or constant-diameter. Refer to

Steady/Transient Treatment of Particles (p. ) for details of these methods.

. If your combusting particle includes an evaporating material, click the Wet Combustion tab, select the

Wet Combustion Model option, and then select the material that is evaporating/boiling from the particle

before devolatilization begins in the Liquid Material drop-down list.You should also set the volume

fraction of the liquid present in the particle by entering the value of the Liquid Fraction. Finally, select

the gas phase species created by the evaporating and boiling laws in the Evaporating Species drop-

down list in the top part of the dialog box.

. If you include multicomponent droplets as the material in your discrete phase model, the Components

tab will become active. In this tab, you will specify the Mass Fraction of each of the components. Note

that the sum of the mass fractions should add up to unity, otherwise ANSYS Fluent will adjust the values

such that you have a sum of  for the mass fraction, and will prompt you to accept the entry. Under

Evaporating Species, select not-vaporizing if the component in the particle does not vaporize. Otherwise,

select the species that will be vaporized.

To change the components of the multicomponent droplet:

a.

In the Create/Edit Materials dialog box, either define a new droplet materials or copy appropriate

materials from the Fluent materials database.

b. Click Edit... next to Mixture Species.

c.

In the Species dialog box, add the droplet materials that you have copied or defined to the Selected

Species list and remove unwanted materials.

. If you want to use a user-defined function to initialize the injection properties, click the UDF tab to access

the UDF inputs.You can select an Initialization function under User-Defined Functions to modify injection

properties at the time the particles are injected into the domain.This allows the position and/or properties

of the injection to be set as a function of flow conditions. More information about user-defined functions

you will need to specify the mass fraction of each particle surface species in the combusting particle.To

do so, click the Multiple Reactions tab, and enter the Species Mass Fractions.These mass fractions refer

to the combustible fraction of the combusting particle, and should sum to . If there is only one surface

species in the mixture material, the mass fraction of that species will be set to , and you will not specify

anything under Multiple Surface Reactions.

Drag and breakup models can be specified on a per-injection basis, allowing you to specify the most

appropriate models for each injection in your model. These per-injection models are specified on the

Physical Models tab of the Set Injection Properties dialog box.

.... Drag Laws

The spherical, nonspherical, Stokes-Cunningham, and high-Mach-number laws described in Particle

Force Balance in the Theory Guide are always available, and the dynamic-drag law described in Dy-

namic Drag Model Theory in the Theory Guide is available only when one of the droplet breakup

models is used in conjunction with unsteady tracking. See Breakup (p. ) for information about en-

abling the droplet breakup models. The Grace and Ishii-Zuber drag laws described in Bubbly Flow

Drag Laws in the Fluent Theory Guide allow to model the drag coefficient in gas-liquid flows in which

the bubbles can have a range of different shapes. Both drag laws are only available if the magnitude

and direction of the gravity vector are specified in the Operating Conditions dialog box. The remaining

three, Wen-Yu, Gidaspow, and Syamlal-OBrien are available only when the dense discrete phase

model is enabled (Including the Dense Discrete Phase Model (p. )) and the flow regime consists

of a dense gas-solid. However, with these models, you cannot verify whether it really is a dense flow

or a gas-solid flow. It is up to you to decide. In any case, these drag formulations are suitable for

dense gas-solid flows.

If the spherical, high-Mach-number, dynamic-drag, Wen-Yu, Gidaspow, or Syamlal-OBrien drag

law is selected, no further inputs are required. If the nonspherical law is selected, the particle Shape

Factor (  in Equation . in the Theory Guide) must be specified. The shape factor value cannot

exceed . For the Stokes-Cunningham law, the Cunningham Correction factor (

in the Theory Guide) must be specified.

.... Particle Rotation

To set-up particle rotation, follow the steps below:

. In the Set Injection Properties dialog box, under the Physical Models tab, enable Particle Rotation.

The options related to the particle rotation feature appear in the Set Injection Properties dialog

box.

. From the Rotational Drag Law drop-down list, select the model for calculating the rotational drag

coefficient

.The following options are available:

Dennis-et-al

Uses Equation . in the Fluent Theory Guide to calculate the rotational drag coefficient

.

none (default)

Implies zero torque, that is, it excludes the influence of the fluid on the rotational particle motion.

. From the Magnus Lift Law drop-down list, select the model for calculating the rotational lift coefficient

.The following models are available:

Oesterle-Bui-Dinh

Uses Oesterle and Bui Dinh’s formulation (Equation . in the Fluent Theory Guide).

Tsuji-et-al

Is based on the particle spin rate (Equation . in the Fluent Theory Guide).

Rubinow-Keller

Uses a linear dependence of the rotational lift coefficient

on the spin rate (Equation . in the

Fluent Theory Guide).

Implies that the Magnus lift will not be included in your simulation.

. Under the Point Properties tab, specify angular velocity components for single, group, and surface

injections; and angular velocity magnitudes for cone injections.

. For each wall with a reflect boundary condition for the discrete phase, specify the friction coefficient (

in Equation . and Equation . in the Fluent Theory Guide) under the DPM tab of the Wall dialog

box. For details, see Friction Coefficient (p. ).

The particle rotation model options are also accessible through the text user interface, under

define/models/dpm/injections/injection-properties/set/physical-mod-

els/particle-rotation. Note that the physical-models command becomes available only

after you have selected the injection(s) using the prompts of the define/models/dpm/injec-

tions/properties/set/pick-injections-to-set text command.

.... Rough Wall Model

To use the rough wall model for walls with the reflect boundary condition type:

.

In the Injection Settings dialog box, under the Physical Models tab, select Rough Wall Model.

.

In the Wall boundary conditions dialog box for the appropriate wall, under the DPM tab, select reflect

from the Boundary Cond.Type drop-down list.

.

Specify the following wall roughness parameters:

Ra

is the wall mean roughness (

Rq

is the standard deviation of the roughness structure (

in Equation . in the Fluent Theory

Guide)

RSm

is the mean roughness slope (the average distance between peaks of wall material) (

in Equa-

tion . in the Fluent Theory Guide)

Note

Guide)

RSm

in Equa-

Note

Note that the DPM Wall Roughness Parameters will only appear in the Wall dialog

box with the reflect DPM boundary condition type if the Rough Wall Model is

selected in the Injection Settings dialog box.

For information about the rough wall model, see Rough Wall Model in the Fluent Theory Guide.

.... Brownian Motion Effects

For sub-micron particles in laminar flow, you may want to include the effects of Brownian motion

(described in Brownian Force in the Theory Guide) on the particle trajectories. To do so, enable the

Brownian Motion option under the Physical Models tab. In order to include Brownian motion effects,

you must also select the Stokes-Cunningham drag law in the Drag Law drop-down list under Drag

Parameters, and specify the Cunningham Correction (

This option is available only when the Energy equation is enabled (in the Models group).

.... Breakup

To enable the modeling of particle breakup for the injection, select Enable Breakup and choose the

Breakup Model (TAB, Wave, KHRT, SSD or Madabhushi) from the drop-down list. A detailed descrip-

tion of these models can be found in Secondary Breakup Model Theory in the Theory Guide.

For the TAB model, you must specify the following values:

y0: Is the initial distortion at time equal to zero (

in Equation . in the Theory Guide).The default

value (

) is recommended.

–

– The number of Breakup Parcels:To split the droplet into several child parcels, as described in Velocity

value (

–

of Child Droplets in the Theory Guide.The diameter of the child parcels is sampled from a Rosin-Rammler

distribution.This can be switched off in the TUI with the command:

/define/models/dpm/spray-model/tab-randomize-breakup-parcel-diameter?

For the Wave model, you must specify the following values:

– B0: Is the constant

– B1: Is the constant

Note

You will generally not need to modify the value of B0, as the default value . is accept-

able for nearly all cases. A value of . is recommended for B1.

The Wave model implementation has been formulated to deal with the initial breakup of a cylindrical

liquid jet. In the Rayleigh regime (that is, at low gas Weber numbers), a cylindrical jet breaks up

into droplets whose diameters are larger than that of the jet itself. In this regime, the model assumes

that the diameter of the continuous, cylindrical liquid jet has been entered as initial diameter in

the injection. Therefore, the droplet diameter can grow beyond the initial diameter. For details, see

Droplet Breakup in the Fluent Theory Guide.

If you want to suppress this feature of the Wave model, use the TUI command:

/define/models/dpm/spray-model/wave-allow-rayleigh-growth? no

Note that this takes effect unconditionally for all injections using the Wave or KHRT breakup

models.

For the KHRT model, you must specify the following values:

– Ctau: Is the constant

– CRT: Is the constant

– CL: :s the constant

The constants B0 and B1 are the same as for the Wave model.

As for the Wave model described above, the KHRT model is formulated to deal with the initial

breakup of a cylindrical liquid jet. The behavior in the Rayleigh regime is as described above for

the Wave model and the same TUI command can be used to modify the behavior. In addition, the

KHRT model uses the Liquid Core Approximation as described in Liquid Core Length in the Fluent

Theory Guide. To suppress the use of the Liquid Core Approximation you can set the Levich constant,

, to zero.

For the SSD model, you must specify the following values:

– Critical We: Is the critical Weber number in Equation . in the Theory Guide.

– Core B1: Is B in Equation . in the Theory Guide.

– Target Np: Is the number of droplets given to each child parcel, before scaling is used to give the correct

overall mass.

– Xi: Is

Note

Xi is a negative value: exp(Xi) is a typical factor by which daughter particles are

smaller than the original parcel.

To set up the Madabhushi breakup model, follow the steps below:

Note

– For the Madabhushi breakup model, the most appropriate injection types are single, group,

and cone (solid-cone).The recommended type is a solid cone injection.

– The Madabhushi breakup model is available only with the dynamic-drag law, which is

automatically selected from the Drag Law drop-down list when the Madabhushi breakup

model is chosen.

. In the Set Injection Properties dialog box, define the Point Properties for the selected injection type

(single, group, or solid cone) as follows:

a.

Specify X-, Y-, and Z- Position  in such a way that the injected droplets build a column over the

midpoint of the nozzle orifice exit.

b. Set Diameter to the jet diameter (nozzle orifice exit diameter).

c.

(single and group injections only) Set X-, Y-, and Z- Velocity  to the inlet velocity components in

x, y, and z directions, respectively.

d. (solid cone injections only) Set Velocity Magnitude and X-, Y-, and Z- Axis to the inlet velocity

magnitude and the direction of the jet, respectively.

e. Set Flow Rate (single and group injections) or Total Flow Rate  (solid cone injections) to the nozzle

orifice flow rate.

f.

(solid cone injections only) Set Cone angle  to  and Outer Radius to the jet radius in order to

specify a perpendicular jet inflow.

g. (solid cone injections only) In the Cone Injector Parameters group box, select Uniform Mass

Distribution.

. In the Physical Models tab, specify the following Madabhushi model parameters:

– For primary breakup based on the Wave breakup model, specify:

→ B0 and B1: Are the same constants as for the Wave model.The recommended values for the

Madabhushi model are B0= . and B1=. See Wave Breakup Model for details about these

→ Jet Diameter: Is the nozzle orifice exit diameter.

– For primary breakup related to the column breakup mechanism, specify:

→ Ligament Factor: Adjusts the diameter of the child droplets arising from the column breakup

mechanism.

→ C0: Is the column breakup time constant that controls how fast the column breakup occurs.The

value recommended for the Madabhushi breakup model is C0=..

. From the Drag Law drop-down list, select dynamic-drag.

The drag is dynamically adapted in the Madabhushi breakup model.

For more information about the Madabhushi breakup model, see Madabhushi Breakup Model in

For steady-state simulations, you also must specify an appropriate Particle Time Step Size and the

Number of Time Steps, which will control the spray density. See Options for Interaction with the

Continuous Phase (p. ) for more information.

Note that you may want to use the dynamic drag law when you use one of the breakup models. See

Drag Laws (p. ) for information about choosing the drag law.

As mentioned in Defining Injection Properties (p. ), you can choose for each injection stochastic

tracking or cloud tracking as the method for modeling turbulent dispersion of particles.

.... Stochastic Tracking

For turbulent flows, if you choose to use the stochastic tracking technique, you must enable the

Discrete Random Walk Model and specify the Number of Tries. Stochastic tracking includes the

effect of turbulent velocity fluctuations on the particle trajectories using the DRW model described

in Stochastic Tracking in the Theory Guide.

. Click the Turbulent Dispersion tab in the Set Injection Properties dialog box.

. Enable stochastic tracking by turning on the Discrete Random Walk Model under Stochastic Tracking.

. Specify the Number of Tries:

Selecting the Turbulent Dispersion model tells ANSYS Fluent to include turbulent velocity fluc-

tuations in the particle force balance as in Equation . in the Theory Guide. The trajectory is

computed more than once if your input exceeds : two trajectory calculations are performed if

you enter , three trajectory calculations are performed if you enter , and so on. Each trajectory

calculation includes a new stochastic representation of the turbulent contributions to the trajectory

equation.

When a sufficient number of tries is requested, the trajectories computed will include a statistical

representation of the spread of the particle stream due to turbulence. Note that for unsteady

particle tracking, the Number of Tries is set to  if using stochastic tracking.

If you want the characteristic lifetime of the eddy to be random (Equation . in the Theory Guide),

enable the Random Eddy Lifetime option. You will generally not need to change the Time Scale

Constant (

in Equation . in the Theory Guide) from its default value of ., unless you are

using the Reynolds Stress turbulence model (RSM), in which case a value of . is recommended.

Figure . : Mean Trajectory in a Turbulent Flow (p. ) illustrates a discrete phase trajectory calcu-

lation computed without turbulent dispersion and Figure . : Stochastic Trajectories in a Turbulent

Flow (p. ) illustrates the “stochastic” tracking (number of tries

) option.

) option.

When multiple stochastic trajectory calculations are performed, the momentum and mass defined

for the injection are divided evenly among the multiple particle/droplet tracks, and are therefore

spread out in terms of the interphase momentum, heat, and mass transfer calculations. Including

turbulent dispersion in your model can thus have a significant impact on the effect of the particles

on the continuous phase when coupled calculations are performed.

Figure . : Mean Trajectory in a Turbulent Flow

Figure . : Stochastic Trajectories in a Turbulent Flow

.... Cloud Tracking

For turbulent flows, you can also include the effects of turbulent dispersion on the injection. Note

that cloud tracking is not available for the massless particle type. When cloud tracking is used, the

trajectory will be tracked as a cloud of particles about a mean trajectory, as described in Particle Cloud

Tracking in the Theory Guide.

. Enable cloud tracking by turning on the Cloud Model under Cloud Tracking.

. Specify the minimum and maximum cloud diameters. Particles enter the domain with an initial cloud

diameter equal to the Min. Cloud Diameter.The particle cloud’s maximum allowed diameter is specified

by the Max. Cloud Diameter.

You may want to restrict the Max. Cloud Diameter to a relevant length scale for the problem to

improve computational efficiency in complex domains where the mean trajectory may become

stuck in recirculation regions.

Important

Important

Note that the cloud model is not available for unsteady particle tracking, and will not allow

you to use the message passing or hybrid option for the particles.

If the standard ANSYS Fluent laws, Laws  through , do not adequately describe the physics of your

discrete phase model, you can modify them by creating custom laws with user-defined functions. More

information about user-defined functions can be found in the Fluent Customization Manual. You can

also create custom laws by using a subset of the existing ANSYS Fluent laws (for example, Laws , ,

and ), or a combination of existing laws and user-defined functions.

Once you have defined and loaded your user-defined function(s), you can create a custom law by en-

abling the Custom option under Laws in the Set Injection Properties Dialog Box (p. ). This will open

the Custom Laws Dialog Box (p. ). In the drop-down list to the left of each of the particle laws, you

can select the appropriate particle law for your custom law. Each list contains the available options

that can be chosen (the standard laws plus any user-defined functions you have loaded).

Figure . : The Custom Laws Dialog Box

There is a final drop-down list in the Custom Laws Dialog Box (p. ) labeled Switching. You may

want to have ANSYS Fluent vary the laws used depending on conditions in the model. You can cus-

tomize the way ANSYS Fluent switches between laws by selecting a user-defined function from this

drop-down list (see DEFINE_DPM_SWITCH in the Fluent Customization Manual).

An example of when you might want to use a custom law might be to replace the standard devolatil-

ization law with a specialized devolatilization law that more accurately describes some unique aspects

of your model. After creating and loading a user-defined function that details the physics of your de-

volatilization law, you would visit the Custom Laws Dialog Box (p. ) and replace the standard devo-

latilization law (Law ) with your user-defined function.

If you have a number of injections for which you want to set the same properties, ANSYS Fluent

provides a shortcut so that you do not need to visit the Set Injection Properties dialog box for each

injection to make the same changes.

As described in Modifying Injections (p. ), if you select more than one injection in the Injections

dialog box, clicking the Set... button will open the Set Multiple Injection Properties dialog box

(Figure . : The Set Multiple Injection Properties Dialog Box (p. )) instead of the Set Injection

Figure . : The Set Multiple Injection Properties Dialog Box

Depending on the type of injections you have selected (single, group, atomizers, and so on), there will

be different categories of properties listed under Injections Setup. The names of these categories

correspond to the headings within the Set Injection Properties dialog box (for example, Particle

Type and Stochastic Tracking). Only those categories that are appropriate for all of your selected in-

jections (which are shown in the Injections list) will be listed. If all of these injections are of the same

type, more categories of properties will be available for you to modify. If the injections are of different

types, you will have fewer categories to select from.

Note

You cannot define any properties as input parameters when you are modifying multiple

injections. If you want to specify a property as an input parameter you must use Fig-

ure . : The Set Injection Properties Dialog Box (p. ).

.... Modifying Properties

To modify a property, perform the following steps:

. Select the appropriate category in the Injections Setup list. For example, if you want to set the same

flow rate for all of the selected injections, select Point Properties.The dialog box will expand to show

the properties that appear under that heading in the Set Injection Properties dialog box.

. Set the property (or properties) to be modified, as described below.

. Click Apply. ANSYS Fluent will report the change in the console window.

Important

You must click Apply to save the property settings within each category. If, for example,

you want to modify the flow rate and the stochastic tracking parameters, you will need

to select Point Properties in the Injections Setup list, specify the flow rate, and click

Apply. You would then repeat the process for the stochastic tracking parameters,

clicking Apply again when you are done.

There are two types of properties that can be modified using the Set Multiple Injection Properties

The first type involves one of the following actions:

selecting a value from a drop-down list

making a selection from a list of radio buttons

The second type involves one of the following actions:

entering a value in a field

enabling / disabling an option

Setting the first type of property works the same way as in the Set Injection Properties dialog box.

For example, if you select Particle Type in the Injections Setup list, the dialog box will expand to

show the portion of the Set Injection Properties dialog box where you choose the particle type.

You can simply choose the desired type and click Apply.

Setting the second type of property requires an additional step. If you select a category in the Injec-

tions Setup list that contains this type of property, the expanded portion of the dialog box will look

like the corresponding part of the Set Injection Properties dialog box, with the addition of Modify

check buttons (see Figure . : The Set Multiple Injection Properties Dialog Box (p. )). To change

one of the properties, first turn on the Modify check button to its left, and then specify the desired

status or value.

For example, if you would like to enable stochastic tracking, first turn on the Modify check button

to the left of Stochastic Model. This will make the property active so you can modify its status. Then,

under Property, turn on the Stochastic Model check button. (Be sure to click Apply when you are

done setting stochastic tracking parameters.)

If you would like to change the value of Number of Tries, select the Modify check button to its left

to make it active, and then enter the new value in the field. Make sure you click Apply when you

have finished modifying the stochastic tracking properties.

Important

The setting for a property that has not been enabled with the Modify check button is not

relevant, because it will not be applied to the selected injections when you click Apply.

After you enable Modify for a particular property, clicking Apply will modify that property

for all of the selected injections, so make sure that you have the settings the way that you

want them before you do this. If you make a mistake, you will have to return to the Set

Injection Properties dialog box for each injection to fix the incorrect setting, if it is not

possible to do so in the Set Multiple Injection Properties dialog box.

.... Modifying Properties Common to a Subset of Selected Injections

Note that it is possible to change a property that is relevant for only a subset of the selected injections.

For example, if some of the selected injections are using stochastic tracking and some are not, enabling

the Random Eddy Lifetime option and clicking Apply will turn this option on only for those injections

that are using stochastic tracking. The other injections will be unaffected.

Simulations of transient particles often require time dependent injection conditions. Potentially most

of the point properties may change over time. One method to accomplish this is the use of an Initial-

ization function as described in DEFINE_DPM_INJECTION_INIT in the Fluent Customization

Manual.

Manual.

An easier way is to use transient profiles containing one or more variables based on the time or crank

angle that can be assigned to various point properties: (Total) Mass Flow Rate, X-, Y-, Z- Velocity,

Velocity Magnitude, and Cone Angle depending on the injection type selected. See Point Properties

for Single Injections (p. ) to Point Properties for Effervescent Atomizer Injections (p. ) for the de-

scription of the individual properties.

Before transient profile variables can be assigned to point properties of injections, a profile file has to

be read into ANSYS Fluent using the File/Read/Profile... ribbon tab item. In the Select File dialog

box a transient profile in tabular format with extension .ttab has to be chosen. Alternatively, you

can read this file into ANSYS Fluent using the read-transient-table text command.

The profile name should not exceed  characters. See Defining Transient Cell Zone and Boundary

Conditions (p. ) for the format description. The following example illustrates an injection within

intervals of . milliseconds injection time, where the second injection has an elevated velocity.

mv-profile

time         mass-flow    velocity

.

. .

. . .

. . .

. .

. .

. .

. .

. .

. .

. . .

. . .

. .

For the setting of point properties go to the Point Properties tab in the Set Injection Properties

When transient profiles are loaded, you can choose either a constant method (the default) or profile

from the Method drop-down list. If you select profile, you also must choose a profile from the corres-

ponding drop-down list that appears in the Value column. The variable angle or time from the file is

used as an independent interpolation variable and cannot be chosen as a profile.

Important

All quantities in the profile file, including coordinate values, must be specified in SI units.

Specifically, Mass Flow Rate must be specified in kg/s, Velocity in m/s, and Cone Angle in

radians. ANSYS Fluent does not perform unit conversion when reading profile files.

When a particle reaches a physical boundary (for example, a wall or inlet boundary) in your model,

ANSYS Fluent applies a discrete phase boundary condition to determine the fate of the trajectory at

that boundary. One of several contingencies may arise:

The particle may be reflected via an elastic or inelastic collision.

The particle may escape through the boundary.The particle is lost from the calculation at the point where

it impacts the boundary.

The particle may be trapped at the wall. Nonvolatile material is lost from the calculation at the point of impact

with the boundary; volatile material present in the particle or droplet is released to the vapor phase at this

point.

The particle may pass through an internal boundary zone, such as radiator or porous jump.

The particle may slide along the wall, depending on particle properties and impact angle.

The particle may form a film (wall film model).

You also have the option of implementing a user-defined function to model the particle behavior when

hitting the boundary. More information about user-defined functions can be found in the Fluent Cus-

tomization Manual.

The boundary condition, or trajectory fate, can be defined separately for each zone in your ANSYS Fluent

model.

... Discrete Phase Boundary Condition Types

... Default Discrete Phase Boundary Conditions

... Coefficients of Restitution

... Friction Coefficient

Setting Boundary Conditions for the Discrete Phase

... Particle-Wall Impingement Heat Transfer

... Film Condensation Model

...Wall Boundary Layer Model

... Setting Particle Erosion and Accretion Parameters

Discrete phase boundary conditions can be set for boundaries in the dialog boxes opened from the

Boundary Conditions task page. When one or more injections have been defined, inputs for the discrete

phase will appear in the dialog boxes. In the Walls dialog boxes, you will need to click the DPM tab

to access the Discrete Phase Model Conditions as shown in Figure . : Discrete Phase Boundary

Conditions in the Wall Dialog Box (p. ).

Figure . : Discrete Phase Boundary Conditions in the Wall Dialog Box

The available boundary conditions are:

reflect

trap

escape

wall-jet

wall-film

interior

Because you can stipulate any of these conditions at flow boundaries, it is possible to incorporate

mixed discrete phase boundary conditions in your ANSYS Fluent model.

Further details are discussed in the following sections:

....The reflect Boundary Condition

....The trap Boundary Condition

....The escape Boundary Condition

....The wall-jet Boundary Condition

....The wall-film Boundary Condition

....The interior Boundary Condition

....The user-defined Boundary Condition

The particle rebounds off the boundary with a change in its momentum. ANSYS Fluent provides two

models for computing this change:

For non-rotating particles, the momentum depends on the coefficient of restitution (Equation . in

the Fluent Theory Guide).

For rotating particles, the model proposed by Tsuji et al. is used.The particle rotation model includes

frictional effects.

The details on these two models can be found in Wall-Particle Reflection Model Theory in the Fluent

For information on how to set up the parameters for non-rotating and rotating particle models, see

Coefficients of Restitution (p. ) and Friction Coefficient (p. ), respectively.

When at least one injection accounts for the rough wall model (the Rough Wall Model option is se-

lected under the Physical Models tab in the Set Injections Properties dialog box), you can specify

the wall surface roughness parameters as described in Rough Wall Model (p. ).

The trajectory calculations are terminated and the fate of the particle is recorded as “trapped”. In the

case of evaporating droplets, their entire mass instantaneously passes into the vapor phase and enters

the cell adjacent to the boundary. See Figure . :“Trap” Boundary Condition for the Discrete

Phase (p. ). In the case of combusting particles, the remaining volatile mass is passed into the vapor

phase.

Figure . : “Trap” Boundary Condition for the Discrete Phase

The particle is reported as having “escaped” when it encounters the boundary in question. Trajectory

calculations are terminated. See Figure . :“Escape” Boundary Condition for the Discrete

Figure . : “Escape” Boundary Condition for the Discrete Phase

The wall-jet type boundary condition is appropriate for high-temperature walls where no significant

liquid film is formed, and in high-Weber-number impacts where the spray acts as a jet. The model is

not appropriate for regimes where film is important (for example, port fuel injection in SI engines,

rainwater runoff, and so on).

A more detailed description of underlying theory is available in Wall-Jet Model Theory in the Theory

Guide.

For the wall-film boundary condition, you can enable and/or set the following models:

Particle impingement/splashing

The following impingement models are available:

– stanton-rutland: (default) consists of four regimes, namely, stick, rebound, spread, and splash, which

are based on the impact energy and wall temperature. See The Stanton-Rutland Model in the Fluent

Theory Guide for more details.

– kuhnke: consists of four regimes spread, rebound, splash, and dry splash (thermal breakup). See The

Kuhnke Model in the Fluent Theory Guide for more details.You must specify the following DPM Wall

Roughness Parameters:

→ Roughness Ra: is used to compute

in Equation . in the Fluent Theory Guide.

→ Roughness Rz: is used to compute splashed droplets ejection angle in Equation . in the Fluent

If you want to model splashing, specify Number of Splash Drops (in the Impingement/Splashing

Model Parameters group box). A value of zero implies that the splashing model will not be used.

The Critical Temperature Factor is used to determine the transition temperature (Equation .

and Equation . in the Fluent Theory Guide for the stanton-rutland and kuhnke splashing

models, respectively).

Film stripping

To model film stripping, enable Particle Stripping and specify Critical Shear Stress (Stripping

Model Parameters group box). When this value is exceeded, mass will be taken from the film on

the face where liquid film exists.

Optionally, you can use the following text user interface commands to specify:

– diameter coefficient (  in Equation . in the Theory Guide (p. )):

define/models/dpm/stripping-options/diameter-coefficient

– mass coefficient (  in Equation . in the Theory Guide (p. )):

define/models/dpm/stripping-options/mass-coefficient

Important

Particle stripping can be modeled only if the film contains a single particle material or

a single particle-mixture material. The combusting-particle type is not supported.

For theoretical information about this option, see Film Stripping in the Fluent Theory Guide.

Film separation

You can select from the following options:

– o'rourke

– o'rourke

– foucart (3d only)

– friedrich.

Details about these models can be found in Separation Criteria in the Fluent Theory Guide.

You can also specify:

– Critical Weber Number: is

in Equation . in the Fluent Theory Guide

– Film Separation Angle: is θcritical in Equation . in the Fluent Theory Guide

Film condensation

See Film Condensation Model (p. ) for details about this mode.

Wall boundary layer model

See Wall Boundary Layer Model (p. ) for details.

Particle erosion (DPM model with the Erosion/Accretion option)

See Setting Particle Erosion and Accretion Parameters (p. ) for details about modeling particle

erosion.

Note

Selecting wall-film automatically enables the Consider Children in the Same Tracking

Step option in the Discrete Phase Model dialog box (Physical Models tab).

Removing the Wall Temperature Limiter for Lagrangian Wall-Film Walls

In ANSYS Fluent, the wall temperature is limited by default. The limit is calculated by Equation .

in the Fluent Theory Guide. You can remove the wall temperature limit by invoking the following text

command:

define/models/dpm/options/remove-wall-film-temperature-limiter?

Remove the wall film temperature limiter [no]: yes

This will result in a smoother wall film appearance. However, since the wall temperature will not be

limited, it may introduce instabilities to the film formation process, and may have the effect that the

wall film completely evaporates off the wall.

If you do use the temperature limit in your simulation, then you have two additional options via the

text user interface (TUI) to define the temperature difference above the Boiling point and disable the

reporting of the Leidenfrost temperature on the wall faces:

define/models/dpm/options/ remove-wall-film-temperature-limiter?

Remove the wall film temperature limiter [no]: no

Temperature difference above the liquid film boiling point []:

Report the Leidenfrost temperature on wall film faces [yes]:

ANSYS Fluent will report in the console the Leidenfrost temperature as a percent of the wall area

covered by film and percent of film mass, where the wall temperature is above the Leidenfrost point.

For more information, see Leidenfrost Temperature Reporting in the Fluent Theory Guide.

Detailed information on the wall film model can be found in Wall-Film Model Theory in the Fluent

For a list of limitations that exist with wall-film boundary conditions, see Limitations on Using the

Lagrangian Wall Film Model (p. ).

The interior boundary condition means that the particles will pass through the internal boundary.

This option is available only for internal boundary zones, such as a radiator or a porous jump.

It is also possible to use a user-defined function to compute the behavior of the particles at a physical

boundary. More information about user-defined functions can be found in the Fluent Customization

Manual.

ANSYS Fluent makes the following assumptions regarding boundary conditions:

Manual.

The reflect type is assumed at wall, symmetry, and axis boundaries, with both coefficients of restitution

equal to .

The escape type is assumed at all flow boundaries (pressure and velocity inlets, pressure outlets, and so

on)

The interior type is assumed at all internal boundaries (radiator, porous jump, and so on)

The coefficient of restitution can be modified only for wall boundaries.

A normal or tangential coefficient of restitution equal to . implies that the particle retains all of its

normal or tangential momentum after the rebound (an elastic collision). A normal or tangential coeffi-

cient of restitution equal to . implies that the particle retains none of its normal or tangential mo-

mentum after the rebound.

Nonconstant coefficients of restitution can be specified for wall zones with the reflect type boundary

condition. The coefficients are set as a function of the impact angle,

, in Particle Reflection at Wall

in the Fluent Theory Guide.

Note that the default setting for both coefficients of restitution is a constant value of . (all normal

and tangential momentum retained).

If you select the reflect type at a wall (only), you can define the Normal and Tangent coefficients of

restitution under Discrete Phase Reflection Coefficients. You can select a constant, polynomial,

piecewise-linear, or piecewise-polynomial function from the relevant drop-down lists. The dialog

boxes for defining the polynomial, piecewise-linear, and piecewise-polynomial functions are the same

as those used for defining temperature-dependent properties. The applied wall heat transfer model

assumes that a liquid is getting in contact with the wall. See Defining Properties Using Temperature-

Dependent Functions (p. ) for details.

When at least one injection accounts for particle rotation (the Enable Rotation option is selected under

the Physical Models tab in the Set Injections Properties dialog box), you can specify friction coeffi-

cients for wall zones with the reflect type boundary condition. In the Wall dialog box, under the DPM

tab, you can define the Friction Coefficient as a constant or as a polynomial, piecewise-linear, or

piecewise-polynomial function.

The default value for the constant is .. For the piecewise-linear and piecewise-polynomial profiles,

the friction coefficient is computed in terms of the relative tangential velocity. The default inputs for

these functions are derived from the friction collision law (The Friction Collision Law in the Fluent

Theory Guide) and are as follows.

The piecewise-linear approximation is defined using the following default points for the relative (particle-

to-wall) tangential velocity:

– Point :  m/s

The piecewise-polynomial approximation is defined in the three relative (particle-to-wall) tangential ve-

locity ranges as follows:

– Range : – m/s: a quadratic function

– Range : – m/s: a constant

– Range : – m/s: a linear function

For details about using the Piecewise-Linear Profile dialog box and Piecewise-Polynomial Profile

dialog box see Inputs for Piecewise-Linear Functions (p. ) and Inputs for Piecewise-Polynomial

Functions (p. ), respectively.

To enable the particle-to-wall heat exchange for the reflect, wall-jet, or wall-film boundary conditions:

In the Wall dialog box, under the DPM tab, enable the Particle-Wall Heat Exchange option. The option

is available only for wall boundary conditions and unsteady particle tracking when the energy equation

Figure . : The Wall Dialog Box: the Particle-Wall Heat Exchange Option

Note that when a particle is reflected from a wall with the wall film DPM boundary condition, the

particle-to-wall heat exchange is calculated directly between the particle and the wall. Any wall film

present is not taken into account.

The model is applied for all inert, droplet, and multicomponent particles impinging on the wall. The

specific model is not applied for the splashed particles. When the wall film DPM boundary condition

is active, the model is applied in the Rebound Regime, and it is assumed that the particles hit the wall

irrespective of the presence of a film. In the Splashing regime, the mass fraction that is deposited

mixes with any existing film, and the splashed particles retain the impinging droplet temperature.

For combusting particles, the wall heat transfer is calculated only if the Wet Combustion Model option

is enabled in the Set Injection Properties dialog box, and the particle liquid fraction is nonzero, oth-

erwise the Particle-Wall Heat Exchange option has no effect.

See Particle–Wall Impingement Heat Transfer Theory in the Fluent Theory Guide for the underlying

theory and equations of the particle–wall impingement heat transfer model.

Condensation can be defined as the transition from the gas phase to the liquid phase as a vapor

condenses on a surface. The ANSYS Fluent film condensation model is triggered when the partial

pressure of vapor species  in the bulk gas mixture exceeds either its vapor pressure at the wall-film

or, in case no film exists, at the wall temperature. When these conditions are met, the vapor species

will condense and form the liquid film on the wall faces.

The following limitations currently exist in the film condensation model:

The film particles are stagnant

Only particles of a single material (droplet or multicomponent) can condense on a particular wall face

At least one species in the mixture must be non-condensable

To use the film condensation model:

. Enable the following models:

Energy equation

Species Transport model

Unsteady Particle Tracking (in the Discrete Phase Model dialog box)

. If no droplet or multicomponent injection exists in the DPM case setup, create a condensate injection by

selecting condensate from the Injection Type dropdown list in the Set Injection Properties dialog box

and define the injection properties as appropriate.

Figure . : The Set Injection Properties Dialog Box: Condensate Injection

Note

A droplet or multicomponent injection must exist to define the vapor–liquid material

pair for the condensation process.

For further information, see Injection Types (p. ), Point Properties for Condensate Injections (p. ),

and Defining Injection Properties (p. ).

. For each droplet and multicomponent injection, specify the condensable species by selecting the Evap-

orating Species.

. In the Wall dialog box, under the DPM tab, select wall-film from the Boundary Cond.Type drop-down

list and enable the Film Condensation option for each wall where condensation may occur.The Fluent

solver automatically enables the Wall Boundary Layer Model. For more information, see Wall Boundary

Layer Model (p. ).

Note

Film Condensation is available only with the wall-film DPM boundary condition.

. Enable Linearized Source Terms in the Numerics tab of the Discrete Phase Model dialog box.

Enabling the Linearized Source Terms option helps to stabilize the condensation solution and is

strongly advisable.

When the appropriate conditions exist, the evaporating species you have selected will condense on

the walls that have the Film Condensation option enabled forming either droplet or multicomponent

film particles (depending on the Particle Type selected in the Set Injection Properties dialog box).

For information about the theory behind the Film Condensation model, see Film Condensation in the

The Wall Boundary Layer model enables the boundary layer formulations for the mass and heat

transfer equations for film vaporization and boiling as described in Film Vaporization and Boiling and

Energy Transfer from the Film in the Fluent Theory Guide.

To enable the model, select Wall Boundary Layer Model in the DPM tab of the Wall dialog box. Note

that the boundary layer formulations are always used for both condensation and vaporization rates

when the Film Condensation model is enabled.

If the Erosion/Accretion option is selected in the Physical Models tab of the Discrete Phase Model

Dialog Box (p. ) (see Monitoring Erosion/Accretion of Particles at Walls (p. )), you can enable

erosion models in the DPM tab of the Wall Dialog Box (p. ) and specify the corresponding erosion

rate parameters at the walls.

Important

The default erosion rate parameters for each erosion model may not be appropriate for

your analysis and must be adjusted based on your own experimental data.

The following models are available in ANSYS Fluent:

Generic Model

The erosion rate of the generic model is defined in Equation . in the Theory Guide as a product

of the mass flux and specified functions for the particle diameter, impact angle, and velocity exponent.

To specify the erosion parameters for the Generic model, click Edit... next to Generic Model.

Figure . : The Generic Erosion Model Parameters Dialog Box

In the Generic Erosion Model Parameters dialog box, specify the following parameters using a

constant, polynomial, piecewise-linear, or piecewise-polynomial function:

– Impact Angle Function:

– Diameter Function:

– Velocity Exponent Function:

See Accretion in the Theory Guide for a detailed description of these functions and Defining Properties

Using Temperature-Dependent Functions (p. ) for details about using the dialog boxes for defining

polynomial, piecewise-linear, and piecewise-polynomial functions.

Finnie

To specify the erosion parameters for the Finnie model, click Edit... next to Finnie.

Figure . : The Finnie Model Parameters Dialog Box

In the Finnie Model Parameters dialog box, specify the following parameters:

– Model Constant, k:

– Velocity Exponent:  in Equation . in the Fluent Theory Guide.The default value is .The value of

the Velocity Exponent is generally within the range of . to . for metals.

– Angle of Maximum Erosion: the impact angle between the approaching particle track and the wall at

which the erosion reaches maximum.

For information about the theory behind the Finnie model, see Finnie Erosion Model in the Fluent

McLaury

To specify the erosion parameters for the McLaury model, click Edit... next to McLaury.

Figure . : The McLaury Model Parameters Dialog Box

In the McLaury Model Parameters dialog box, specify the following parameters:

– Model Constant, A:

– Velocity Exponent:

– Transition Angle:

in Equation . and Equation . in the Fluent Theory Guide.

– Impact Angle Constant, b:  in Equation . in the Fluent Theory Guide.

– Impact Angle Constant, c:  in Equation . in the Fluent Theory Guide.

– Impact Angle Constant, w:

– Impact Angle Constant, x:  in Equation . in the Fluent Theory Guide.

– Impact Angle Constant, y:

See Example of the McLaury Erosion Model Constants in the Fluent Theory Guide for more information

about the McLaury model parameters. For theoretical background on the McLaury model, see McLaury

Erosion Model in the Fluent Theory Guide.

Oka

To specify the erosion parameters for the Oka model, click Edit... next to Oka.

Figure . : The Oka Model Parameters Dialog Box

In the Oka Model Parameters dialog box, specify the following parameters:

– Reference Erosion Rate:

– Wall Material Hardness:

– Model Constant, n1:

– Model Constant, n2:

– Diameter Exponent:

– Reference Diameter:

– Reference Velocity:

See Example of the Oka Erosion Model Constants in the Fluent Theory Guide for an example of the

Oka model parameters' values. For more information on the theory behind the Oka model, see Oka

Shear Stress (dense flows with the disperse granular phase only)

To specify the erosion parameters for the shear stress model, click Edit... next to Shear Stress.

Figure . : The Shear Stress Model Parameters Dialog Box

In the Shear Stress Model Parameters dialog box, specify the following parameters:

– Velocity Exponent:  in Equation . in the Fluent Theory Guide.

– Empirical Model Constant:

– Solid Phase Packing Limit:

This model should be used for dense multiphase flow with a dispersed phase consisting of solid

particles. For more information on the theory behind the shear stress model, see Abrasive Erosion

Caused by Solid Particles in the Fluent Theory Guide.

Granular Phase Shielding (dense flows with the disperse granular phase only)

The granular phase shielding as given by Equation . in the Fluent Theory Guide is always con-

sidered in the shear stress erosion model. If you want to include the shielding effect in other erosion

models that are currently enabled, select Granular Phase Shielding. This option is available only

when Shear Stress Model Parameters is selected.

For more information about the theory behind the wall shielding effects in dense flows, see Wall

Shielding Effect in Dense Flow Regimes in the Fluent Theory Guide.

By default, all erosion models are enabled.

Important

The default constants for the Finnie, Oka, and McLaury models have been tuned to match the

experiment described by Oka [] (p. ) in which -micron sand particles impact a carbon

steel wall at a speed of  m/s and therefore are only valid for those specific conditions.You

can use the default values as a starting point for your simulation and then adjust them as needed.

Predictive capabilities of the erosion models are limited and strongly case dependent.

Under certain circumstances, it is desirable to compute not only the particle-induced wall erosion rates,

but also the actual deformation of the material due to erosion. The erosion of material from the surface

of the wall may create large cavities that will affect particulate flow and erosion processes and eventually

lead to material failure. To account for changes in the wall's shape and position and for more accurate

predictions of the erosion rates, ANSYS Fluent provides the capability to couple the erosion rate solver

with the dynamic mesh model.

Generally, erosion is a slow process, typically far slower than the processes on the fluid side. ANSYS

Fluent implements the erosion dynamic mesh model using a quasi-steady approach. During each step

of the solution process, the flow and particle erosion simulations are performed as steady-state,

whereas the mesh position is updated by the dynamic mesh module using the physical time step size.

When erosion is coupled with dynamic meshes, ANSYS Fluent computes the mesh deformation of an

individual face

as:

(.)

where,

= Wall face specific erosion rate density

= Mesh motion time step

= Wall material density

Before setting up a calculation of erosion coupled with the dynamic mesh model, perform the following

steps:

. Set up a DPM case (including defining fluid properties, setting boundary and cell zone conditions,

steps:

etc.). For information on setting up a DPM calculation, see Steps for Using the Discrete Phase Models

in the Fluent User's Guide (p. ).

. Set up injections as described in Creating and Modifying Injections in the Fluent User's Guide (p. ).

. Create report definitions to monitor flow variables.

. Specify convergence criteria and solver controls for your simulation.

. Initialize the flow field and run the solution.

Note that you need to compute a large number of particle trajectories in order to provide

sufficiently smooth erosion patterns for the dynamic mesh motion algorithm.

. Enable erosion/accretion on affected walls as described in Monitoring Erosion/Accretion of Particles

at Walls (p. ) and Setting Particle Erosion and Accretion Parameters in the Fluent User's Guide (p. ).

Once erosion/accretion is enabled, the Erosion Dynamic Mesh item appears in the tree under

the Setup/Models/Discrete Phase tree branch.

Particle Erosion Coupled with Dynamic Meshes

. Perform a calculation for the erosion rates.

Note

Note that it is not necessary to initialize the flow field and calculate both flow and

erosion prior to coupling erosion with dynamic mesh. However, it will speed up

the erosion dynamic mesh simulation if you start from a converged flow field and

then follow with a first estimation of the erosion rates.

. Once the solution is completed, select Steady in the Genteral task page (Solver group).

Note

Erosion coupling with dynamic mesh is available only for steady-state flows due to being

implemented via a quasi-steady approach.

You must run the erosion dynamic mesh simulation from the Erosion Dynamic Mesh

Coupling Setup dialog box only, and not from the Run Calculation task page or by

using text commands.

... Procedure for the Erosion Coupled with Dynamic Mesh Setup and

Solution

. Open the Erosion Dynamic Mesh Coupling Setup dialog box and select Enable Erosion Dynamic Mesh

Coupling.

Setup → Models → Discrete Phase → Erosion Dynamic Mesh

Edit...

Figure . : The Erosion Dynamic Mesh Coupling Setup Dialog Box

. In the Erosion Settings group box, select an appropriate Reference Erosion Model for your simulation

and specify the Wall Material Density.

You can choose from the following erosion models:

finnie (default)

generic-model

mclaury

oka

For information about these models, refer to Setting Particle Erosion and Accretion Parameters in

Note that these models will not be available if you are using a UDF to specify the erosion accretion

rates as described in DEFINE_DPM_EROSION in the Fluent Customization Manual. In this case,

only udf will appear in Reference Erosion Model.

The wall material density is assumed to be identical for all walls involved in the erosion coupled

with dynamic mesh simulation. Note that for Wall Material Density, you may need to adjust the

default value of  kg/m3, which is the density of aluminum.

. (dense flows with the disperse granular phase only) If you want to model abrasive erosion rates and wall

shielding effects, select Include Abrasive Erosion Effects. For more information about these models,

refer to Modeling Erosion Rates in Dense Flows in the Fluent Theory Guide.

. In the Dynamic Mesh Settings group box, you can:

Specify a non-zero value for # of Smoothing Steps if you want to apply smoothing to the wall erosion

rates in the dynamic mesh module.

Smoothing the erosion rates is recommended. For cases with a lower particle count, you can

increase the # of Smoothing Steps to a value greater than . Note that tracking a sufficient

number of particles in your simulation will ensure no large variations in erosion rate density. If

you refine your mesh by a factor of  in each direction, you also need to increase the number

of particles by a factor of  or more.

Enable Automatic Dynamic Mesh Setup (default)

The Automatic Dynamic Mesh Setup allows for a quick setup of the basic functionalities needed

for an erosion dynamic mesh coupled simulation. Selecting this option automatically enables

Dynamic Mesh and the smoothing, local cell remeshing, local face remeshing, and face region

remeshing methods. These methods will ensure that the mesh quality remains acceptable during

the simulation. The option also automatically creates a dynamic zone of a User-Defined type

for each zone participating in the coupled erosion dynamic mesh simulation. The motion of the

dynamic zones is defined by the **erosion** mesh motion UDF provided by ANSYS Fluent.

– Specifying the Motion of Dynamic Zones (p. )

– User-Defined Motion (p. )

– Smoothing Methods (p. )

– Local Cell Remeshing Method (p. )

– Local Remeshing Method (p. )

– Face Region Remeshing Method (p. )

The automatic dynamic mesh setup uses the dynamic mesh methods with reasonable defaults,

which may not be optimal for all cases. If you want to modify the dynamic mesh settings after

the automatic setup has been completed, you must first disable Automatic Dynamic Mesh

Setup; otherwise, your changes will be overwritten by the default settings. Before adjusting the

dynamic mesh settings, you should become familiar with the Deform Adjacent Boundary Layer

with Zone and Feature Detection options, which are described in Boundary Layer Smoothing

Method (p. ) and Feature Detection in the Fluent User's Guide (p. ).

. From the Participating Walls selection list, select walls that will be deformed due to particle-wall erosion.

. To set controls for the erosion dynamic mesh solver and then run the simulation, click Run Erosion-Dy-

namic Mesh Simulation….

Figure . : The Run Erosion-Dynamic Mesh Simulation Dialog Box

a.

In the Mesh Motion Time Setup group box, you can select the time stepping method to compute

the mesh deformation from Equation . (p. ):

fixed-time-step: allows you to specify a constant Time Step.

variable-time-step (default): is automatically determined by the dynamic mesh solver based

on the following parameters:

Maximum Node Movement (% of Wall Face Length Scale)

the maximum allowed cell deformation per meshing step. It is specified as a fraction (in

percent) of the characteristic length, which is derived from the cell wall face area. A default

of % is an acceptable, conservative value. To speed up the calculation, you can set this

parameter to a higher value. A value of  to %, or even higher, is suitable in most

cases. However, because the erosion rate is considered to be constant during each time

step, some erosion rate variations may be lost for larger mesh deformations. Trial and

error may be required to find an optimal value for your case input.

Minimum/Maximum Time Step Size

upper and lower time limits. If you want the solver to use the time step calculated by

the dynamic mesh module, set Maximum Time Step Size to a large value.

During the iteration process, the solver adjusts the time step based on the maximum

node movement. The solver will gradually increase the time step up to its maximum

value, resulting in a faster overall simulation time. ANSYS Fluent will report the time step

used in the current iteration in the console and in the Time Step field.

b. In the Simulation Termination group box, specify the Total Time of Erosion (in seconds).The simu-

lation stops when the specified time period ends.

c.

In the Flow Simulation Control group box, you can specify:

Iterations per Flow Simulation: is the number of flow iterations between mesh deformation steps.

This number should be sufficiently large to ensure that the flow simulation converges between

successive mesh steps.

(only when Interaction with Continuous Phase is enabled) Solve DPM during Flow Simulation:

enforces a tighter coupling between gas and particle phases. During the flow calculation, the particle

tracker will be called regularly at the frequency specified in DPM Iteration Interval in the Discrete

Phase Model dialog box.

d. If you want to automatically save case and data files during the calculation, you can specify a filename

and a frequency with which case and data files should be saved for postprocessing or restart purposes

in the Autosave Files group box.When saving case and data files, ANSYS Fluent appends the filename

that you have provided with @time=flow time .

e. Specify the autosave plot options in the Autosave Graphics group box.

i.

If you want to capture images of mesh, contour, or vector plots at the specified intervals for later

use (for example, to generate animations of your solution over time), set the frequency at which

your plots will be saved in the Save Plots Every text entry field and click Select Graphics....

Note

The Select Graphics... button becomes available only after the flow field has

been initialized.

Figure . : The Graphics Objects Dialog Box

A. In the Graphics Objects dialog box, from the New Object drop-down list, select the object

that you want to save:

Mesh... opens the Mesh Display Dialog Box (p. )

Contours... opens the Contours Dialog Box (p. )

Vectors... opens the Vectors Dialog Box (p. )

Once you create a new object, it will be displayed in the Graphics Objects dialog box.

B. Select which graphics objects you want to save as PNG images during the solution run. Similar

to case and data files, the image filenames will be appended with @time=flow time .

ii.

If you want ANSYS Fluent to plot the vertex maximum of the accumulated deformation variable

on all walls undergoing mesh deformation, enable Automatic Mesh Deformation Report.

ii.

When you start iterating, ANSYS Fluent automatically creates the max-accumulated-deform-

ation report definition and max-accumulated-deformation-pset report plot, which will be

displayed in the graphics window during the solution run.

. Click Run... in the Run Erosion-Dynamic Mesh Simulation dialog box.

Important

The erosion dynamic mesh simulation must be run only from the Run Erosion-Dynamic

Mesh Simulation dialog box.

During the coupled erosion dynamic mesh analysis, first, the erosion module computes erosion

rates and passes them to the dynamic mesh module. The dynamic mesh module performs a pseudo-

steady simulation of the mesh deformation. After that, the solver carries out a steady-state flow

calculation for a specified number of flow iterations. If Solve DPM during Flow Simulation is en-

abled, the particle tracking is performed in the specified DPM Iteration Interval. Otherwise, the

particle tracker is run once after the flow calculation is finished. Whenever the particle tracker is

run, the DPM sources are updated. This process is repeated until the specified Total Time Of

Erosion is reached.

As the solution progresses, ANSYS Fluent reports the dynamic mesh time step and the simulation

time in the console and the Time Step and Elapsed Simulation Time fields. If you interrupt the

simulation using the Interrupt Simulation dialog box, the solver will complete the current flow

and erosion iterations before stopping the calculation.

... Postprocessing for Erosion Dynamic Mesh Calculations

You can generate graphical plots or alphanumeric reports for the mesh deformation using the following

additional postprocessing variable:

Accumulated Deformation (in the Mesh... category)

In order to apply the physical models described in earlier sections to the prediction of the discrete

phase trajectories and heat/mass transfer, ANSYS Fluent requires many physical property inputs.

... Summary of Property Inputs

... Setting Discrete-Phase Physical Properties

Table . : Property Inputs for Inert Particles (p. ) – Table . : Property Inputs for Multicomponent

Particles (Law ) (p. ) summarize which of these property inputs are used for each particle type and

in which of the equations for heat and mass transfer each property input is used. Detailed descriptions

of each input are provided in Setting Discrete-Phase Physical Properties (p. ).

Table . : Property Inputs for Inert Particles

Symbol

Property

in Equation . in the Theory Guide

density

in Equation . and Equation .

particle emissivity

particle scattering factor

thermophoretic coefficient

Table . : Property Inputs for Droplet Particles

Symbol

Properties

density

viscosity

Symbol

in Equation ., Equation .,

Equation ., and Equation .

viscosity

Symbol

latent heat

vaporization temperature

in Equation ., Equation .

boiling point

volatile component fraction

binary diffusivity

diffusivity reference pressure

saturation vapor pressure

heat of pyrolysis

droplet surface tension

composition averaging coefficient

temperature averaging coefficient

Thermolysis model

– single-rate

in Equation . (droplet material) or

in

Equation . in the Fluent Theory Guide

(multicomponent particles)

pre-exponential factor

in

activation energy

– constant

in

rate constant

Table . : Property Inputs for Combusting Particles (Laws –)

Symbol

Property

density

Setting Material Properties for the Discrete Phase

Symbol

Property

swelling coefficient

burnout stoichiometric ratio

combustible fraction

heat of reaction for burnout

Symbol

Property

fraction of reaction heat given to solid

devolatilization model

– law , constant rate

– – constant

– law , single rate

– – pre-exponential factor

– – activation energy

– law , two rates

– – pre-exponential factors

– – activation energies

– – weighting factors

– law , CPD

– – initial fraction of bridges in coal lattice

– – initial fraction of char bridges

– – lattice coordination number

– – cluster molecular weight

in

– – side chain molecular weight

Table . : Property Inputs for Combusting Particles (Law )

Symbol

Property

combustion model

– law , diffusion rate

– – binary diffusivity

– – diffusivity reference pressure

– law , diffusion/kinetic rate

– – mass diffusion limited rate constant

– – kinetics limited rate pre-exp. factor

Symbol

Property

– – kinetics limited rate activation energy

– law , intrinsic rate

– – kinetics limited rate active energy

– – char porosity

– – mean pore radius

– – specific internal surface area

– – tortuosity

– – burning mode

Table . : Property Inputs for Multicomponent Particles (Law )

Symbol

Property

selected droplets for components

mixture species

in Equation . of the Theory Guide

density

vapor particle equilibrium

....The Concept of Discrete-Phase Materials

When you create a particle injection and define the initial conditions for the discrete phase (as de-

scribed in Setting Initial Conditions for the Discrete Phase (p. )), you choose a particular material

as the particle’s material. All particle streams of that material will have the same physical properties.

Important

Note that you will not choose a Material for a Massless particle type in the Set Injections

Discrete-phase materials are divided into four categories, corresponding to the four types of particles

available. These material types are inert-particle, droplet-particle, combusting-particle, and mul-

ticomponent-particle. Each material type will be added to the Material Type list in the Create/Edit

Materials Dialog Box (p. ) when an injection of that type of particle is defined (in the Set Injection

Properties or Set Multiple Injection Properties dialog box, as described in Setting Initial Conditions

for the Discrete Phase (p. )). The first time you create an injection of each particle type, you will

be able to choose a material from the database, and this will become the default material for that

type of particle. That is, if you create another injection of the same type of particle, your selected

material will be used for that injection as well. You may choose to modify the predefined properties

for your selected particle material, if you want (as described in Modifying Properties of an Existing

Material (p. )). If you need only one set of properties for each type of particle, you need not define

any new materials; you can simply use the same material for all particles.

Important

If you do not find the material you want in the database, you can select a material that is

close to the one you want to use, and then modify the properties and give the material a

new name, as described in Creating a New Material (p. ).

Important

Note that a discrete-phase material type will not appear in the Material Type list in the

Create/Edit Materials dialog boxes until you have defined an injection of that type of

particles. This means, for example, that you cannot define or modify any combusting-

particle materials until you have defined a combusting particle injection (as described in

Setting Initial Conditions for the Discrete Phase (p. )).

For a particle-mixture material type, you must select the species in your mixture. To do this, click

the Edit... button next to Mixture Species in the Create/Edit Materials dialog box. The Species

dialog box will open, where you will include your Selected Species. The selected species will now

be available in the Set Injection Properties dialog box, under the Components tab (Figure . : The

Components Tab (p. )).

Figure . : The Components Tab

..... Defining Additional Discrete-Phase Materials

In many cases, a single set of physical properties (density, heat capacity, and so on) is appropriate

for each type of discrete phase particle considered in a given model. Sometimes, however, a single

model may contain two different types of inert, droplet, combusting particles, or multicomponent

particles (for example, heavy particles and gaseous bubbles or two different types of evaporating

liquid droplets). In such cases, it is necessary to assign a different set of properties to the two (or

more) different types of particles. This is easily accomplished by defining two or more inert, droplet,

or combusting particle materials and using the appropriate one for each particle injection.

You can define additional discrete-phase materials either by copying them from the database or by

creating them from scratch. See Using the Create/Edit Materials Dialog Box (p. ) for instructions

on using the Create/Edit Materials Dialog Box (p. ) to perform these actions.

Important

Recall that you must define at least one injection (as described in Setting Initial Conditions

for the Discrete Phase (p. )) containing particles of a certain type before you will be

Important

able to define additional materials for that particle type.

.... Description of the Properties

The properties that appear in the Create/Edit Materials Dialog Box (p. ) vary depending on the

particle type (selected in the Set Injection Properties or Set Multiple Injection Properties dialog

box, as described in Defining Injection Properties (p. ) and Defining Properties Common to More

than One Injection (p. )) and the physical models you are using in conjunction with the discrete-

phase model.

All properties you may need to define for a discrete-phase material are listed below (alphabetically).

See   Table . : Property Inputs for Inert Particles (p. ) – Table . : Property Inputs for Combusting

Particles (Law ) (p. ) to see which properties are defined for each type of particle.

Binary Diffusivity

is the mass diffusion coefficient used in the vaporization law (Law ),

in

Equation . in the Theory Guide.This input is also used to define the mass diffusion of the oxidizing

species to the surface of a combusting particle,

, as given in Equation . in the Theory Guide.

(Note that the diffusion coefficient inputs that you supply for the continuous phase are not used for the

discrete phase.)

For Droplet Particle type Materials, select film-averaged from the Binary Diffusivity drop-down

list and specify parameters for the film-averaged model (see Equation . in the Theory Guide)

using the Film Binary Diffusivity dialog box. The film-averaged model is recommended when

accurate temperature-dependent binary diffusivity data are available.

To apply the unity Lewis number model (Equation . in the Fluent Theory Guide) select unity-

lewis-number from the Binary Diffusivity drop-down. The unity Lewis number model is a sim-

plified approach and is not appropriate when the molecular weights of the evaporating species

(or oxidizing species for combusting particles) and the gas-phase mixture are very different. The

model can be applied, for example, for the evaporation of water, light hydrocarbons, or methanol

in air, but is not appropriate for heavy hydrocarbons.

You also have the option of implementing a user-defined function to model the particle binary

diffusivity. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more information.

To enable the pressure dependence for the binary diffusivity, in the Create/Edit Materials dialog

box, under Properties, from the Diffusivity Reference Pressure drop-down list, select constant

(see Equation . in the Fluent Theory Guide) and enter a value for the reference pressure

that corresponds to the value defined for the Binary Diffusivity material property. The pressure

dependence option is available with all property methods for the binary diffusivity, including

user-defined, with the exception of the unity Lewis number model, for which the pressure de-

pendence is already accounted for through the density variable in the model equation.

Boiling Point

is the temperature,

, at which the calculation of the boiling rate equation (Equation . in the

Theory Guide) is initiated by ANSYS Fluent.When a droplet particle reaches the boiling point, ANSYS

Fluent applies Law  and assumes that the droplet temperature is constant at

.The boiling point

denotes the temperature at which the particle law transitions from the vaporization law to the boiling

law.

For multicomponent particles the boiling point of the components is used only as a reference

temperature of the latent heat. Instead, the boiling starts when the sum of the partial component

saturation pressures reach the total fluid pressure. The definition of the saturation pressure curve

is therefore essential for the boiling of multicomponent particles.

You also have the option of implementing a user-defined function to model the particle boiling

point. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more information.

Burnout Stoichiometric Ratio

is the stoichiometric requirement,

, for the burnout reaction, Equation . in the Theory Guide, in

terms of mass of oxidant per mass of char in the particle.

Combustible Fraction

is the mass fraction of char,

, in the coal particle, that is, the fraction of the initial combusting particle

that will react in the surface reaction, Law  (Equation . in the Theory Guide).

Combustion Model

defines which version of the surface char combustion law (Law5) is being used.You can choose from

the following options:

diffusion-limited (default)

The binary diffusivity defined above will be used in Equation . in the Theory Guide.

kinetics/diffusion-limited

When the kinetics/diffusion-limited limited rate model is selected for the surface combustion

model, the Kinetics/Diffusion-Limited Combustion Model Dialog Box (p. ) opens where you

can enter the Mass Diffusion Limited Rate Constant (

Guide), Kinetics Limited Rate Pre-exponential Factor (

in Equation . ), and Kinetics

Limited Rate Activation Energy (  in Equation . ).

Note that the Kinetics/Diffusion-Limited Combustion Model dialog box is a modal dialog

box, which means that you must tend to it immediately before continuing the property defini-

tions.

intrinsic-model

When the intrinsic-model is selected for the surface combustion model, the Intrinsic Combustion

Model Dialog Box (p. ) opens where you can enter the Mass Diffusion Limited Rate Constant

(

in Equation . in the Theory Guide), Kinetics Limited Rate Pre-exponential Factor (

in Equation . ), Kinetics Limited Rate Activation Energy (

in Equation . ), Char

Porosity (  in Equation . ), Mean Pore Radius (

in Equation . ), Specific Internal

Surface Area (

in Equation . Equation . ), Tortuosity (  in Equation . ), and

Burning Mode, alpha (  in Equation . ).

Note that the Intrinsic Combustion Model dialog box is a modal dialog box, which means

that you must tend to it immediately before continuing the property definitions.

multiple-surface-reactions

When multiple-surface-reactions is selected, ANSYS Fluent displays the Multiple Surface Reac-

tions Dialog Box (p. ) informing you to open the Reactions dialog box, where you can review

or modify the particle surface reactions that you specified as described in Overview of User Inputs

for Modeling Species Transport and Reactions (p. ). In addition, you can set property options

for the char specific heat and density:

Composition Dependent Specific Heat

if this option is enabled, your input for the particle

property will be used to determine

the specific heat of the volatiles and ash component only. The specific heat of the char will

be calculated as a mass-weighted average of the particle surface species specific heat values,

and the particle specific heat is finally calculated as the mass average of the char and

volatiles+ash fractions. The specific heat of the particle surface species should be defined

in the corresponding fluid materials of the Mixture material.

Composition Dependent Density

if this option is enabled, your input for the particle Density property will be used to determ-

ine the density of the volatiles and ash component. The density of the char will be calculated

as a volume-weighted average value of the particle surface species densities, and the particle

density is finally calculated as the volume-weighted average of the char and volatiles+ash

fractions. The density of the particle surface species should be defined in the corresponding

fluid materials of the Mixture material.

Important

If you have not yet defined any particle surface reactions, you must be sure to define

them now. See Using the Multiple Surface Reactions Model for Discrete-Phase Particle

Important

Combustion (p. ) for more information about using the multiple surface reactions

model.

You will notice that the Burnout Stoichiometric Ratio and Heat of Reaction for Burnout are

no longer available in the Create/Edit Materials dialog box, as these parameters are now

computed from the particle surface reactions you defined in the Reactions dialog box.

Note that the multiple surface reactions model is available only if the Particle Surface option

for Reactions is enabled in the Species Model dialog box. See User Inputs for Particle Surface

Reactions (p. ) for details.

Composition Averaging Coefficient,

is the coefficient

in Equation . in the Fluent Theory Guide.To assume bulk gas composition for

the physical properties in the particle vaporization and heating rates equations, select none from the

Composition Averaging Coefficient drop-down in the Create/Edit Materials dialog box, under

Properties.To enable property averaging, select constant and enter a value between  and  for the

Composition Averaging Coefficient.

=  corresponds to bulk gas mixture. For

= , the composition

reverts to the particle surface composition.

Important

When you define the Composition Averaging Coefficient with a constant value

other than , you must also specify Specific Heat, Viscosity and Thermal Conductivity

for the evaporating species (in the Create/Edit Materials dialog box, under Properties,

for the corresponding fluid material of the continuous phase mixture). Note that for

the definition of the evaporating species properties, the user-defined method is not

supported and should not be used.

The default and recommended value for the averaging coefficient is /. However, to improve

the simulation results, you must provide accurate temperature-dependent data for the vapor

material (through the Create/Edit Materials dialog box).

Cp

is the specific heat,

, of the particle.The specific heat may be defined as a function of temperature by

selecting one of the function types from the drop-down list to the right of Cp. See Defining Properties

Using Temperature-Dependent Functions (p. ) for details about temperature-dependent properties.

For multicomponent particles, it can be calculated as a mass-weighted value of the specific heat of the

droplet component.

You also have the option of implementing a user-defined function to model the particle specific

heat. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more information.

A composition-dependent char specific heat option can be enabled if you are using the multiple-

surface-reactions model for a combusting particle. For details on enabling this model, see Com-

bustion Model

(p. ).

When you are using the non-premixed or the partially-premixed combustion model in the con-

tinuous phase calculation, the specific heat defined for the particle material will be used for the

specific heat and enthalpy calculations of the non-volatile/non-reacting particle mass.

Density

is the density of the particulate phase in units of mass per unit volume of the discrete phase.This density

Density

is the mass density and not the volumetric density.The density may be defined as a function of temper-

ature by selecting one of the function types from the drop-down list to the right of Density. See Defining

Properties Using Temperature-Dependent Functions (p. ) for details about temperature-dependent

properties. For compressible flows, or if any of the real-gas models is enabled, the compressible-liquid

method is also available. See Compressible Liquid Density Method (p. ) for details. For multicomponent

particles, it can be calculated as a volume-weighted value of the density of the droplet components.

You also have the option of implementing a user-defined function to model the particle density.

See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more information.

For a combusting particle that swells during the trajectory calculations, the temperature-dependent

density calculation is suspended during the devolatilization law and your input is used to determine

the initial particle diameter,

at the start of the devolatilization in Equation . in the Fluent

Theory Guide. A composition-dependent char density option can be enabled if you are using the

multiple-surface-reactions model for a combusting particle. For details on enabling this model,

see Combustion Model

(p. ).

Devolatilization Model

defines which version of the devolatilization model, Law , is being used.

You can choose the following devolatilization models (as described in Devolatilization (Law ) in

the Theory Guide):

constant (default)

To use the default constant rate devolatilization model (as described in Equation . in the

Theory Guide), enter the rate constant

in the field below the list.

single rate

When the single kinetic rate model is selected, the Single Rate Model Dialog Box (p. ) opens

where you can enter the Pre-exponential Factor,

, and the Activation Energy,

, to be used

in Equation . in the Theory Guide for the computation of the kinetic rate.

two-competing-rates

When the two competing rates model (two-competing-rates) is selected, the Two Competing

Rates Model Dialog Box (p. ) opens where you can enter, for the First Rate and the Second

Rate, the Pre-exponential Factor (

Theory Guide), Activation Energy (

in Equation . ), and

Weighting Factor (

and

in Equation . ). The constants you specify are used in Equa-

tion . through Equation ..

cpd-model

When the CPD model (cpd-model) is selected, the CPD Model dialog box opens where you

can enter the Initial Fraction of Bridges in Coal Lattice (

in Equation . of the Theory

Guide), Initial Fraction of Char Bridges (

in Equation . ), Lattice Coordination Number

(

in Equation . ), Cluster Molecular Weight (

in Equation . ), and Side Chain

Molecular Weight (

Note that the Single Rate Model, Two Competing Rates Model, and CPD Model dialog boxes

are modal dialog boxes, which means that you must tend to them immediately before continuing

the property definitions.

Diffusivity Reference Pressure

is the reference pressure

for the pressure dependent binary diffusivity in Equation . in the

Fluent Theory Guide.To apply the pressure dependence, in the Create/Edit Materials dialog box, under

Properties, from the Diffusivity Reference Pressure drop-down list, select constant and enter a refer-

ence pressure value corresponding to the value for the Binary Diffusivity material property. If none is

selected from the Diffusivity Reference Pressure drop-down list, ANSYS Fluent assumes no pressure

dependence for the binary diffusivity.

Heat of Pyrolysis

is the heat of the instantaneous pyrolysis reaction ,

, that the evaporating/boiling species may un-

dergo when released to the continuous phase.This input represents the conversion of the evaporating

species to lighter components during the evaporation process.The heat of pyrolysis should be specified

as a positive number for exothermic reaction and as a negative number for endothermic reaction.The

default value of zero implies that the heat of pyrolysis is not considered.This input is used in Equa-

tion . in the Theory Guide.

Heat of Reaction for Burnout

is the heat released by the surface char combustion reaction, Law  (Equation . in the Theory

Guide).This parameter is specified in terms of heat release (for example, Joules) per unit mass of char

consumed in the surface reaction.

Latent Heat

is the latent heat of vaporization,

, required for phase change from an evaporating liquid droplet

(Equation ., Equation ., Equation ., and Equation . in the Theory Guide) or for the

evolution of volatiles from a combusting particle (Equation . in the Theory Guide).This input is

supplied in units of J/kg in SI units or of Btu/

in British units and is treated as a constant by ANSYS

Fluent. For the droplet particle, the latent heat value at the boiling point temperature should be used.

You also have the option of implementing a user-defined function to model the particle latent

React. Heat Fraction Absorbed by Solid

(Equation . in the Theory Guide), which controls the distribution of the heat

of reaction between the particle and the continuous phase.The default value of zero implies that the

entire heat of reaction is released to the continuous phase.

Saturation Vapor Pressure

is the saturated vapor pressure,

, defined as a function of temperature, which is used in the vaporiz-

ation law, Law  (Equation . in the Theory Guide).The saturated vapor pressure may be defined

as a function of temperature by selecting one of the function types from the drop-down list to the right

of its name. (See Defining Properties Using Temperature-Dependent Functions (p. ) for details about

temperature-dependent properties.) In the case of unrealistic inputs, ANSYS Fluent restricts the range

of

to between . and the operating pressure. Correct specification of a realistic vapor pressure

curve is essential for accurate results from the vaporization model.

You also have the option of implementing a user-defined function to model the particle saturation

vapor pressure. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more in-

Swelling Coefficient

in Equation . in the Theory Guide, which governs the swelling of the coal

particle during the devolatilization law, Law  (Devolatilization (Law ) in the Theory Guide). A swelling

coefficient of unity (the default) implies that the coal particle stays at constant diameter during the de-

volatilization process.

You also have the option of implementing a user-defined function to model the particle swelling

coefficient. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more information.

Temperature Averaging Coefficient,

in Equation . in the Fluent Theory Guide.To assume bulk gas temperature for

Temperature Averaging Coefficient drop-down in the Create/Edit Materials dialog box, under

Temperature Averaging Coefficient.

=  corresponds to bulk gas conditions. For

= , the temper-

ature reverts to the particle surface temperature.

Important

When you define the Temperature Averaging Coefficient with a constant value

other than , you must also define Specific Heat, Viscosity and Thermal Conductivity

the simulation results, you must provide accurate temperature-dependent data for the evaporating

vapor material (through the Create/Edit Materials dialog box).

is the thermal conductivity of the particle,

.This input is specified in units of W/m-K in SI units or

in British units and is treated as a constant by ANSYS Fluent.

Thermolysis Model

defines which Thermolysis model is used for the calculation of the mass transfer of the vaporizing species

from the droplet to the bulk phase according to a Thermolysis rate equation.You can choose from the

following options:

single-rate

When single-rate is selected, the Single Rate Model Dialog Box (p. ) opens where you specify

the Pre-exponential Factor

and the Activation Energy

to be used in Equation . (if

you are modelling a droplet material), or the Pre-exponential Factor

and Activation Energy

in Equation . in the Fluent Theory Guide (if you are modelling multicomponent particles).

constant

For the constant rate Thermolysis model, enter the rate constant  to be used in Equation .

(if you are modelling a droplet material), or the rate constant

in Equation . in the Fluent

Theory Guide (if you are modelling multicomponent particles).

none (default) signifies that the Thermolysis rate model is disabled.

Note that if you are using a multicomponent particle, the Thermolysis model is set for the indi-

vidual droplet materials. A typical application is the modeling of Selective Catalytic Reduction

(SCR) systems where it is recommended to use the single-rate Thermolysis model for the urea-liquid

component in the urea-water particle mixture.

Thermophoretic Coefficient

in Equation . in the Theory Guide, and appears when the thermophoretic

force (which is described in Thermophoretic Force in the Theory Guide) is included in the trajectory

calculation (that is, when the Thermophoretic Force option is enabled in the Discrete Phase Model

dialog box).The default is the expression developed by Talbot  [] (p. ) (talbot-diffusion-coeff)

and requires no input from you.You can also define the thermophoretic coefficient as a function of

temperature by selecting one of the function types from the drop-down list to the right of Thermophor-

etic Coefficient. See Defining Properties Using Temperature-Dependent Functions (p. ) for details

about temperature-dependent properties.

You also have the option of implementing a user-defined function to model the particle thermo-

phoretic coefficient. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more

information.

Vaporization Temperature

, at which the calculation of vaporization from a liquid droplet or devolatilization

from a combusting particle is initiated by ANSYS Fluent. Until the particle temperature reaches

, the

particle is heated via Law , Equation . in the Theory Guide.This temperature input represents a

modeling decision rather than any physical characteristic of the discrete phase.

You also have the option of implementing a user-defined function to model the particle vaporiz-

ation temperature. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more

Vapor-Particle-Equilibrium

is the selected approach for the calculation of the vapor concentration of the components at the surface.

This can be Raoult’s law (Equation . in the Theory Guide), the Peng-Robinson real gas model

(Equation . in the Theory Guide), or a user-defined function that defines the equilibrium.

Vaporization/Boiling Model

defines which vaporization/boiling model is used for pure droplets (Law ) and for multicomponent

droplets (Law ).You can choose from the following options:

diffusion-controlled (default)

This option will apply Equation . in the Theory Guide.

convection/diffusion-controlled

When you select the convection/diffusion-controlled model for vaporization, Equation .

in the Theory Guide will be applied for the calculation of the vaporization rate, and Equa-

tion . in the Theory Guide will be applied in the particle heat transfer calculations This

model is recommended when evaporation rates are high. For slowly evaporating droplets both

models are expected to give similar results.

Once you have selected convection/diffusion-controlled, you can enable the Variable Lewis

Number Formulation option in the Model Options dialog box to compute the Spalding heat

number from Equation . in the Fluent Theory Guide. If the option is disabled ANSYS Fluent

uses Equation ..

You can also enable averaging of the Spalding heat transfer term for the convection/diffusion-

controlled model according to Equation . in the Fluent Theory Guide by using the TUI

command define/models/dpm/options/vaporization-heat-transfer-aver-

aging. This option has the net effect of increasing the heat-transfer to the droplet and may

produce more realistic results for cases with large temperature differences between droplet

and bulk gas.

For both diffusion-controlled and convection/diffusion-controlled models, you can select Use the

Specific Heat of the Evaporating Species in Boiling Law in the Model Options Dialog Box (p. ).

This option sets the heat capacity of the gas (

to the specific heat of the evaporating species selected in the Set Injection Properties dialog

box. For the convection/diffusion controlled model with the Variable Lewis Number Formulation,

this option is selected by default. This ensures consistency with the convection/diffusion controlled

model expression for

Volatile Component Fraction

(

) is the mass fraction of a droplet particle that may vaporize via Laws  and/or  (Droplet Vaporization

(Law ) in the Theory Guide). For combusting particles, it is the mass fraction of volatiles that may be

evolved via Law  (Devolatilization (Law ) in the Theory Guide).

When the effect of particles on radiation is enabled (for the P- or discrete ordinates radiation model

only) in the Discrete Phase Model Dialog Box (p. ), you must define the following additional para-

meters:

Particle Emissivity

is the emissivity of particles in your model,

, used to compute radiation heat transfer to the particles

meters:

(Equation ., Equation ., Equation ., Equation ., and Equation . in the Theory

Guide) when the P- or discrete ordinates radiation model is active. Note that you must enable radiation

to particles, using the Particle Radiation Interaction option in the Discrete Phase Model Dialog

Box (p. ). Recommended values of particle emissivity are . for coal particles and . for ash  [] (p. ).

You also have the option of implementing a user-defined function to model the particle

emissivity. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more information.

Particle Scattering Factor

is the scattering factor,

, due to particles in the P- or discrete ordinates radiation model (Equation .

in the Theory Guide). Note that you must enable particle effects in the radiation model, using the Particle

Radiation Interaction option in the Discrete Phase Model Dialog Box (p. ).The recommended value

of

for coal combustion modeling is . [] (p. ). Note that if the effect of particles on radiation is

enabled, scattering in the continuous phase will be ignored in the radiation model.

You also have the option of implementing a user-defined function to model the particle scattering

factor. See DEFINE_DPM_PROPERTY in the Fluent Customization Manual for more information.

When an atomizer injection model and/or the droplet breakup or collision model is enabled in the

Set Injection Properties Dialog Box (p. ) (atomizers) and/or Discrete Phase Model Dialog Box (p. )

(droplet breakup/collision), you must define the following additional parameters:

is the droplet surface tension,

.The surface tension may be defined as a function of temperature by

selecting one of the function types from the drop-down list to the right of Droplet Surface Tension.

See Defining Properties Using Temperature-Dependent Functions (p. ) for details about temperature-

dependent properties.You also have the option of implementing a user-defined function to model the

droplet surface tension. More information about user-defined functions can be found in the Fluent

Viscosity

is the droplet viscosity,

.The viscosity may be defined as a function of temperature by selecting one

of the function types from the drop-down list to the right of Viscosity. See Defining Properties Using

Temperature-Dependent Functions (p. ) for details about temperature-dependent properties.You

also have the option of implementing a user-defined function to model the droplet viscosity. More in-

formation about user-defined functions can be found in the Fluent Customization Manual.

Solution of the discrete phase implies integration in time of the force balance on the particle (Equa-

tion . in the Theory Guide) to yield the particle trajectory. As the particle is moved along its trajectory,

heat and mass transfer between the particle and the continuous phase are also computed via the

heat/mass transfer laws (Laws for Heat and Mass Exchange in the Theory Guide). The accuracy of the

discrete phase calculation therefore depends on the time accuracy of the integration and upon the

appropriate coupling between the discrete and continuous phases when required. Numerical controls

are described in Numerics of the Discrete Phase Model (p. ). Coupling and performing trajectory

calculations are described in Performing Trajectory Calculations (p. ). Resetting the Interphase Exchange

Terms (p. ) and Parallel Processing for the Discrete Phase Model (p. ) provide information about

resetting interphase exchange terms and using the parallel solver for a discrete phase calculation.

... Performing Trajectory Calculations

... Resetting the Interphase Exchange Terms

The trajectories of your discrete phase injections are computed when you display the trajectories using

graphics or when you perform solution iterations. That is, you can display trajectories without impacting

the continuous phase, or you can include their effect on the continuum (termed a coupled calculation).

In turbulent flows, trajectories can be based on mean (time-averaged) continuous phase velocities or

they can be impacted by instantaneous velocity fluctuations in the fluid. This section describes the

procedures and commands you use to perform coupled or uncoupled trajectory calculations, with or

without stochastic tracking or cloud tracking.

.... Uncoupled Calculations

For the uncoupled calculation, you will perform the following two steps:

. Solve the continuous phase flow field.

. Plot (and report) the particle trajectories for discrete phase injections of interest.

In the uncoupled approach, this two-step procedure completes the modeling effort, as illustrated in

Figure . : Uncoupled Discrete Phase Calculations (p. ). The particle trajectories are computed

as they are displayed, based on a fixed continuous-phase flow field. Graphical and reporting options

are detailed in Postprocessing for the Discrete Phase (p. ).

Figure . : Uncoupled Discrete Phase Calculations

This procedure is adequate when the discrete phase is present at a low mass and momentum loading,

in which case the continuous phase is not impacted by the presence of the discrete phase.

.... Coupled Calculations

In a coupled two-phase simulation, ANSYS Fluent modifies the two-step procedure above as follows:

. Solve the continuous phase flow field (prior to introduction of the discrete phase).

. Introduce the discrete phase by calculating the particle trajectories for each discrete phase injection.

. Recalculate the continuous phase flow, using the interphase exchange of momentum, heat, and mass

determined during the previous particle calculation.

. Recalculate the discrete phase trajectories in the modified continuous phase flow field.

. Repeat the previous two steps until a converged solution is achieved in which both the continuous phase

flow field and the discrete phase particle trajectories are unchanged with each additional calculation.

This coupled calculation procedure is illustrated in Figure . : Coupled Discrete Phase Calcula-

tions (p. ). When your ANSYS Fluent model includes a high mass and/or momentum loading in the

discrete phase, the coupled procedure must be followed in order to include the important impact of

the discrete phase on the continuous phase flow field.

Solution Strategies for the Discrete Phase

Figure . : Coupled Discrete Phase Calculations

Important

When you perform coupled calculations, all defined discrete phase injections will be

computed. You cannot calculate a subset of the injections you have defined. If there are

massless particle injections defined, these will have no effect in the coupled calculation.

..... Procedures for a Coupled Two-Phase Flow

If your ANSYS Fluent model includes prediction of a coupled two-phase flow, you should begin with

a partially (or fully) converged continuous-phase flow field. You will then create your injection(s)

and set up the coupled calculation.

For each discrete-phase iteration, ANSYS Fluent computes the particle/droplet trajectories and updates

the interphase exchange of momentum, heat, and mass in each control volume. These interphase

exchange terms then impact the continuous phase when the continuous phase iteration is performed.

During the coupled calculation, ANSYS Fluent will perform the discrete phase iteration at specified

intervals during the continuous-phase calculation. The coupled calculation continues until the con-

tinuous phase flow field no longer changes with further calculations (that is, all convergence criteria

are satisfied). When convergence is reached, the discrete phase trajectories no longer change either,

since changes in the discrete phase trajectories would result in changes in the continuous phase

flow field.

The steps for setting up the coupled calculation are as follows:

. In the Discrete Phase Model Dialog Box (p. ) (Figure . :The Discrete Phase Model Dialog Box and

the Tracking Parameters (p. )), enable the Interaction with Continuous Phase option.

. Set the frequency with which the particle trajectory calculations are introduced in the DPM Iteration

Interval field. If you set this parameter to , for example, a discrete phase iteration will be performed

every fifth continuous phase iteration.The optimum number of iterations between trajectory calculations

depends upon the physics of your ANSYS Fluent model.

Important

Note that if you set this parameter to , ANSYS Fluent will not perform any discrete

phase iterations.

During the coupled calculation (which you initiate using the Run Calculation Task Page (p. ) in

the usual manner) you will see the following information in the ANSYS Fluent console as the continu-

ous and discrete phase iterations are performed:

iter   continuity   x-velocity   y-velocity       k         epsilon       energy    time/it

.5249e-   .8657e-   .0533e+   .6227e-   .9771e-   .8181e-   ::

.7955e-   .5867e-   .2736e-   .4516e-   .6545e-   .2314e-   ::

DPM  Iteration  ....

number  tracked=  ,  number  escaped=  ,  aborted=  ,  trapped=  ,  evaporated  =  ,i

Done.

.9206e-   .1860e-   .9573e-   .2692e-   .3997e-   .4532e-   ::

.0729e-   .2982e-   .3036e-   .1649e-   .2111e-   .5369e-   ::

.2820e-   .5508e-   .0900e-   .9018e-   .6619e-   .0394e-   ::

Done.

Note that you can perform a discrete phase calculation at any time by using the solve/dpm-update

text command.

..... Stochastic Tracking in Coupled Calculations

If you include the stochastic prediction of turbulent dispersion in the coupled two-phase flow calcu-

lations, the number of stochastic tries applied each time the discrete phase trajectories are introduced

during coupled calculations will be equal to the Number of Tries specified in the Set Injection

Properties Dialog Box (p. ). For transient particle tracking, the number of tries is set to . Input of

this parameter is described in Stochastic Tracking (p. ). An input of

requests  stochastic

trajectory calculations for each particle in the injection. When the number of stochastic tracks included

is small, you may find that the ensemble average of the trajectories is quite different each time the

trajectories are computed. These differences may, in turn, impact the convergence of your coupled

solution. For good convergence of a coupled solution, a statistical independent distribution of tracks

can be achieved with an adequate number of stochastic tracks and/or a sufficient number of different

starting locations of the tracks.

..... Under-Relaxation of the Interphase Exchange Terms

When you are coupling the discrete and continuous phases using the calculation procedures noted

above, ANSYS Fluent applies under-relaxation to the momentum, heat, and mass transfer terms. This

under-relaxation serves to increase the stability of the coupled calculation procedure by letting the

impact of the discrete phase change only gradually:

(.)

where

is the exchange term,

is the previous value,

is the newly computed value,

and  is the particle/droplet under-relaxation factor. For , ANSYS Fluent uses a default value of .

for all types of analysis except transient flows with unsteady particle tracking, in which case the default

value of . is used. You can modify  by changing the value in the Discrete Phase Sources field

under Under-Relaxation Factors in the Solution Controls task page. You may need to decrease

in order to improve the stability of coupled discrete phase calculations.

Figure . : Effect of Number of Source Term Updates on Source Term Applied to Flow Equa-

tions (p. ) shows how the source term , when applied to the flow equations, changes with the

number of updates for varying under-relaxation factors . Each DPM iteration starts with an initial

value for the source term, which is typically zero at the beginning of the calculation. After a

number of updates, the source term reaches its final

value.

Figure . : Effect of Number of Source Term Updates on Source Term Applied to Flow

Equations

Suppose that in a continuous flow simulation with continuous DPM tracking, the DPM under-relaxation

factor is chosen to be ., with  continuous phase iterations per DPM iteration. From Figure . : Ef-

fect of Number of Source Term Updates on Source Term Applied to Flow Equations (p. ), we see

that approximately  source term updates are required for the DPM sources to reach their final

values. Therefore, in this example, at least  continuous phase iterations are required after any

change to the DPM sources (for example, a new injection or a changed DPM mass flow rate), to ensure

that the change has taken effect.

For cases with convergence difficulties, reducing the under-relaxation factors is often necessary in

order to improve the stability of the coupled DPM simulation. However, for small values of , many

iterations may be needed for the DPM source to reach the final

value. You can use a text command

that linearly ramps up the DPM source term to its maximum

value. At the end of each iteration

, the source term is computed as:

With this approach, even small values for under-relaxation factors can be applied, and the final

value can be reached within a reasonable iteration count. For the above example, a minimum of

two source term updates is required to reach the final values. Accordingly, it will take only  con-

tinuous phase iterations to fully account for the effect of the DPM source changes.

To use the linear growth of DPM source term functionality, use the following text commands:

define/models/dpm/interaction/linear-growth-of-dpm-source-term?

Change the DPM source term linearly every DPM iteration [no] y

Note that the impact of this option is case dependent.

If you have performed coupled calculations, resulting in nonzero interphase sources/sinks of momentum,

heat, and/or mass that you do not want to include in subsequent calculations, you can reset these

sources to zero.

Reset DPM Sources

When you select Reset DPM Sources, the sources will immediately be reset to zero without any further

confirmation from you.

After you have completed your discrete phase inputs and any coupled two-phase calculations of interest,

you can display and store the particle trajectory predictions. ANSYS Fluent provides both graphical and

alphanumeric reporting facilities for the discrete phase, including the following:

graphical display of the particle trajectories

summary reports of trajectory fates

step-by-step reports of the particle position, velocity, temperature, and diameter

alphanumeric reports and graphical display of the interphase exchange of momentum, heat, and mass

optionally, alphanumeric reports and graphical display of various cell-averaged discrete phase field variables

sampling of trajectories at boundaries and lines/planes

summary reporting of current particles in the domain

histograms of trajectory data at sample planes

display of erosion/accretion rates

exporting of trajectories to Fieldview and Ensight

This section provides detailed descriptions of each of these postprocessing options.

(Note that plotting or reporting trajectories does not change the source terms.)

... Displaying of Trajectories

... Reporting of Trajectory Fates

... Step-by-Step Reporting of Trajectories

... Reporting of Current Positions for Unsteady Tracking

... Reporting of Interphase Exchange Terms (Discrete Phase Sources)

... Reporting of Discrete Phase Variables

... Reporting of Unsteady DPM Statistics

... Sampling of Trajectories

... Histogram Reporting of Samples

Postprocessing for the Discrete Phase

... Summary Reporting of Current Particles

... Postprocessing of Erosion/Accretion Rates

... Assessing the Risk for Solids Deposit Formation During Selective Catalytic Reduction Process

When you have defined discrete phase particle injections, as described in Setting Initial Conditions for

the Discrete Phase (p. ), you can display the trajectories of these discrete particles using the Particle

Tracks Dialog Box (p. ) (Figure . : The Particle Tracks Dialog Box (p. )).

You can create named particle track definitions and save them for later use. See Creating and Using Contour

Plot Definitions (p. ) for additional information on graphics object definitions.

Note that particle track definitions can be included in scenes as long as the XY Plot option is not enabled.

See Displaying a Scene (p. ) for additional information on scenes.

Edit...

You can also crate a named particle track plot definition and save it for later use.

New...

Figure . : The Particle Tracks Dialog Box

The procedure for drawing trajectories for particle injections is as follows:

. Select the particle injection(s) you want to track in the Release from Injections list. (You can choose to

track a specific particle, instead, as described below.)

. If you have not done this yet, set the Step Length Factor and the Max. Number of Steps (Tracking tab)

in the Discrete Phase Model Dialog Box (p. ).

Edit...

If stochastic and/or cloud tracking is desired, set the related parameters in the Set Injection

Properties dialog box, as described in Stochastic Tracking (p. ).

Note

Displaying tracks multiple times at the same solution state will result in identical

random tracks. This is because the same seeding is used enabling you to postprocess

different variables on the same particle tracks.

. (optional) Specify which particles you want to display.

a.

If you want to display a single particle stream, enable Track Single Particle Stream and specify the

particle stream ID number in the Stream ID field.

Note

To determine the stream ID in the injection of interest, use the Injections Dialog Box (p. )

to list the injection particle streams, as described in Listing Injections (p. ).The stream

ID numbers will be listed in the first column of the data printed in the ANSYS Fluent con-

sole.

For unsteady tracking, all of the particles related to the specified injection stream will be

displayed.The displayed data will not correspond to the time history of an individual

particle.

b. (wall film model only) Enable Free Stream Particles and/or Wall Film Particles if you want to display

those types of particles. Note that these options are available only when the Lagrangian wall film

model is enabled in the wall boundary conditions dialog box, under the DPM tab.

. Set any of the display options described below.

. Click the Display (or Save/Display) button to draw the trajectories or click the Pulse button to animate

the particle positions.The Pulse button will become the Stop ! button during the animation, and you

must click Stop ! to stop the pulsing.

Important

For unsteady particle tracking simulations, clicking Display will show only the current location

of the particles.Typically, you should select point in the Track Style drop-down list when

displaying transient particle locations since individual positions will be displayed.

The Pulse button option is not available for unsteady tracking.

.... Options for Particle Trajectory Plots

You can include the mesh in the trajectory display, control the style of the trajectories (including the

twisting of ribbon-style trajectories), color them by different scalar fields and control the color scale,

and coarsen trajectory plots. (More information about these options can be found in Controlling the

Particle Tracking Style (p. ) and Controlling the Vector Style of Particle Tracks (p. ).) You can also

choose node or cell values for display. If you are “pulsing” the trajectories, you can control the pulse

mode. Finally, you can generate an XY plot of the particle trajectory data (for example, residence

time) as a function of time or path length and save this XY plot data to a file.

Note

The Draw Mesh option settings are not saved with the particle track plot definition. Once

the dialog box is closed these settings will revert to being disabled. If you want these

settings persisted within the current session, you can use the non-persistent Particle Tracks

Results → Graphics → Particle Tracks → Edit...

Plotting particle trajectories can be very time consuming, therefore, to reduce the plotting time, a

coarsening factor can be used to reduce the number of points that are plotted. Providing a coarsening

factor of , will result in each

th point being plotted for a given trajectory in any cell. This coarsening

factor is specified in the Particle Tracks Dialog Box (p. ), in the Coarsen field and is only valid for

steady-state cases. For example, if the coarsening factor is set to , then ANSYS Fluent will plot alternate

points.

Important

Note that if any particle or pathline enters a new cell, this point will always be plotted.

To reduce plotting time in transient cases, ANSYS Fluent has available an option to skip plotting every

particle in an injection. Selecting this option is also done in the Particle Tracks Dialog Box (p. )

by specifying a nonzero integer in the Skip field. For example, if an individual stream is selected and

the skip option is set to , every other particle will be plotted. If the entire injection is selected with

a skip option of , every other particle will be plotted for all streams in the injection.

These options are controlled in exactly the same way that pathline-plotting options are controlled.

See Options for Pathline Plots (p. ) for details about setting the trajectory plotting options mentioned

above.

Note that in addition to coloring the trajectories by continuous phase variables, you can also color

them according to the following discrete phase variables: particle time, particle velocity, particle dia-

meter, particle density, particle mass, particle temperature, particle law number, particle time step,

and particle Reynolds number. If DEM Collisions is enabled in the Discrete Phase Model dialog box,

you can also select the magnitude or components of the collisional force acting on the DEM parcel,

total force acting on the DEM parcel, and total acceleration experienced by the particles in the parcel.

These variables are included in the Particle Variables... category of the Color by list. To display the

minimum and maximum values in the domain, click the Update Min/Max button.

.... Controlling the Particle Tracking Style

Particle tracking can be displayed as lines (with or without arrows), ribbons, cylinders (coarse, medium,

or fine), triangles, spheres, or a set of points. In the Track Style drop-down list in the Particle Tracks

dialog box, you can choose:

(steady tracking) line, line-arrows, point, sphere, ribbon, triangle, coarse-cylinder, medium-cylinder,

or fine-cylinder.

(unsteady tracking) point or sphere.

Pulsing can be done only on point, sphere, or line styles.

Once you have selected the track style, click the Attributes... button to specify how you would like

to display the particle tracks.

Note

The Track Style options that will appear depend on whether you are running a tran-

sient or steady-state simulation. For a transient case, the only Track Style options

available are the point and sphere styles.

If you are using the line or line-arrows style, set the Line Width in the Track Style Attributes dialog box

(Figure . :The Track Style Attributes Dialog Box (p. )) that appears when you click the Attributes...

button. For line-arrows you will also set the Spacing Factor, which controls the spacing between the

particles tracks.The size of the arrow heads can be adjusted by entering a value in the Scale text-entry

box.

Figure . : The Track Style Attributes Dialog Box

If you are using the point style, you will set the Marker Size in the Track Style Attributes dialog box.

The thickness of the particle track will be the thickness of the marker.

If you are using the sphere style, you will set the Diameter, scale, and Detail in the Particle Sphere Style

Attributes dialog box (Figure . :The Particle Sphere Style Attributes Dialog Box (p. )).You have the

option of specifying a constant diameter if you enable Constant under Options and you will then specify

the Diameter. If you enable Variable, you can select a particle variable to estimate the size of the spheres.

The spheres are scaled by the factor entered in the Scale entry box.

The best constant diameter to use will depend on the dimensions of the domain, the view, and

the particle density. However, an adequate starting point would be a diameter on the order of /

of the average cell size or / step size. Units for the Diameter field correspond to the mesh dimen-

sional units.

The level of detail applied to the graphical rendering of the spheres can be controlled using the

Detail field. The level of detail uses integer values ranging from  to . Note that the performance

of the graphical rendering as well as the memory consumption will be better when using a small

level of detail, that is, very coarse spheres, such as  or . The rendering performance significantly

decreases with higher levels of detail. You should gradually increase the detail to determine the

best-case scenario between performance and quality.

Whenever Auto Range is disabled, the spheres are displayed only if they have values between Min

and Max.

Also note that to take full advantage of spherical rendering, lighting should be turned on in the

view. The Gouraud setting provides much smoother looking spheres than the Flat setting and

better performance than the Phong setting. For more information on lighting, see Adding

Lights (p. ).

Figure . : The Particle Sphere Style Attributes Dialog Box

If you are using the triangle or any of the cylinder styles, you will set the Width in the Track Style Attrib-

utes dialog box. For triangles, the specified value will be half the width of the triangle’s base, and for cyl-

inders, the value will be the cylinder’s radius.

If you are using the ribbon style, clicking on the Attributes... button will open the Ribbon Attributes

Dialog Box (p. ), in which you can set the ribbon’s Width.You can also specify parameters for twisting

the ribbon tracks. In the Twist By drop-down list, you can select a scalar field on which the tracks twisting

is based (for example, helicity). Select the desired category in the upper list and then select a related

quantity in the lower list.The twisting may not be displayed smoothly because the scalar field by which

you are twisting the tracks is calculated at cell centers only (and not interpolated to a particle’s position).

The Twist Scale sets the amount of twist for the selected scalar field.To magnify the twist for a field with

very little change, increase this factor; to display less twist for a field with dramatic changes, decrease this

factor.

When you click Compute, the Min and Max fields will be updated to show the range of the Twist

By scalar field.

.... Controlling the Vector Style of Particle Tracks

You can choose to have the particle tracks displayed as vectors. Choose the Vector Style from the

drop-down list in the Particle Tracks dialog box:

If you select vector, the vector will be generated starting in the center of the particle, as shown in

Figure . : Particles with the Vector Style (p. ).

If you select centered-vector, the midpoint of the vector will appear in the center of the particle, as

shown in Figure . : Particles with the Centered Vector Style (p. ).

If you select centered-cylinder, the midpoint of the cylinder will appear in the center of the particle,

as shown in Figure . : Particles with the Centered Cylinder Style (p. ).

Figure . : Particles with the Vector Style

Figure . : Particles with the Centered Vector Style

Figure . : Particles with the Centered Cylinder Style

Click the Attributes... button to specify how you would like to display the particle tracks. In the

Particle Vector Style Attributes dialog box (Figure . : The Particle Vector Style Attributes Dialog

Box (p. )) you will set the Length, Scale, and Length to Head Ratio. The direction of the vectors

is displayed for the selected variable under Vectors of. You have the option of specifying a Constant

Length or a Variable Length, which is based on the variable selected under Length by. If Constant

Color is enabled, then all vectors/cylinders are colored by the color selected in the Color drop-down

list. Otherwise, it is the color selected in the Particle Tracks dialog box (seen in the Mesh Colors

dialog box when Draw Mesh is enabled).

Vectors can be scaled by the factor given in the Scale entry box. The ratio of vector length to vector

head size can be changed in the box Length to Head Ratio. In the case of a cylinder, the ratio of

the length to the diameter is affected.

Figure . : The Particle Vector Style Attributes Dialog Box

.... Importing Particle Data

Use the Import Particle Data dialog box (Figure . : The Import Particle Data Dialog Box (p. ))

to import particle data to display in the graphics window.

Results → Model Specific → Discrete Phase → Import Particle Data...

Figure . : The Import Particle Data Dialog Box

. Click Read... to display a file selection dialog box where you can enter a file name and a directory that

contains the imported data.

. Choose from the available import options by selecting Auto Range and/or Draw Mesh under Options.

If you prefer to restrict the range of the scalar field, disable the Auto Range option and set the Min and

Max values manually beneath the Color by list.

. Choose to color the particle pathlines by any of the scalar fields in the Color by list. If you select COLORBY,

the pathlines will be colored by the quantity that was chosen when the particle data file was created.

(See Exporting Steady-State Particle History Data (p. ))

. Select a pathline style under Style.To set pathline style attributes, click the Attributes... button. For

more information about the pathline style types, see Controlling the Pathline Style (p. ).

. The value of Steps sets the maximum number of steps a particle can advance. A particle will stop when

it has traveled this number of steps or when it leaves the domain.

. If your pathline plot is difficult to understand because there are too many paths displayed, you can “thin

out” the pathlines by changing the Skip value.

. Click the Display button to draw the pathlines, or click the Pulse button to animate the particle positions.

The Pulse button will become the Stop ! button during the animation, and you must click Stop ! to stop

the pulsing.

.... Particle Filtering

You can specify how you would like to filter the particles being displayed, by first enabling the Filter

option, then clicking the Filter by... button. In the Particle Filter Attributes dialog box, select the

field variable by which you want to filter, then specify whether you would like to display all the particle

tracks Inside or Outside the Filter-Min and Filter-Max range, as shown in Figure . : The Particle

Filter Attributes Dialog Box (p. ).

Note

Note

All particle variables as well as any field variable except for Custom Field Functions... can

be used as a filter variable.

Figure . : The Particle Filter Attributes Dialog Box

.... Graphical Display for Axisymmetric Geometries

For axisymmetric problems in which the particle has a nonzero circumferential velocity component,

the trajectory of an individual particle is often a spiral about the centerline of rotation. ANSYS Fluent

displays the  and  components of the trajectory (but not the  component) projected in the

axisymmetric plane.

When you perform trajectory calculations by displaying the trajectories (as described in Displaying of

Trajectories (p. )), ANSYS Fluent will provide information about the trajectories as they are completed.

By default, the number of trajectories with each possible fate (escaped, aborted, evaporated, and so

on) is reported:

DPM Iteration ....

num. tracked = , escaped = , aborted = , trapped = , evaporated = , inco

Done.

You can also track particles through the domain without displaying the trajectories by clicking the

Track button at the bottom of the dialog box. This allows the listing of reports without also displaying

the tracks.

....Trajectory Fates

The possible fates for a particle trajectory are as follows:

“Escaped” trajectories are those that terminate at a flow boundary for which the “escape” condition is set.

“Incomplete” trajectories are those that were terminated when the maximum allowed number of time

steps — as defined by the Max. Number of Steps input in the Discrete Phase Model Dialog Box (p. )

(see Numerics of the Discrete Phase Model (p. )) — was exceeded.

“Incomplete_parallel” may appear as an additional fate for parallel simulations.This means that the

number of particle exchanges between partitions has been exceeded. Any remaining particles on the

compute nodes are stopped, which is indicated by the number following this fate.Therefore no further

source terms from these particles are considered.The number of particle exchanges is limited to avoid

very long computational time due to incomplete particles.You can change the default value of  to

a value of  with a scheme command. Contact the technical support engineer for this information.

“Trapped” trajectories are those that terminate at a flow boundary where the “trap” condition has been

set.

“Evaporated” trajectories include those trajectories along which the particles were evaporated within the

domain.

“Aborted” trajectories are those that fail to complete due to roundoff reasons.You may want to retry the

calculation with a modified length scale and/or different initial conditions.

“Shed” trajectories are newly generated particles during the breakup of a larger droplet.They appear only

if a breakup model is enabled.

“Coalesced” trajectories are removed particles which have coalesced after particle-particle collisions.They

appear only if the coalescence model is enabled.

“Splashed” trajectories are particles that are newly generated when a particle touches a wall film.Those

trajectories appear only if the wall film model is enabled.

.... Summary Reports

You can request additional detail about the trajectory fates as the particles exit the domain, including

the mass flow rates through each boundary zone, mass flow rate of evaporated droplets, and com-

position of the particles.

. Follow steps  and  in Displaying of Trajectories (p. ) for displaying trajectories.

. Select Summary as the Report Type and click Display or Track.

Important

For steady-state simulations, DPM summary data is not stored in the .dat file, since

it is possible to track particles on single or combinations of injections. Transient simu-

lations store this data since it is accumulated over time starting from initialization.

A detailed report similar to the following example will appear in the console window. (You may also

choose to write this report to a file by selecting File as the Report to option, clicking the Write...

button (which was originally the Display button), and specifying a file name for the summary report

file in The Select File Dialog Box (p. ).)

number  tracked  =  ,  escaped  =  ,  aborted  =  ,  trapped  =  ,  evaporated  =  ,

Fate             Number                    Elapsed  Time  (s)

Min            Max            Avg        Std  Dev

----              ------     ----------     ----------     ----------      ----------

Evaporated                   .770e-     .114e-     .456e-      .686e-

Escaped  -  Zone            .043e-     .037e-     .471e-      .172e-

Trapped  -  Zone            .486e-     .767e-     .030e-      .421e-

(*)-  Mass  Transfer  Summary  -(*)

Fate                         Mass  Flow  (kg/s)

Initial          Final          Change

----                    ----------     ----------      ----------

Evaporated              .333e-     .000e+     -.333e-

Escaped  -  Zone       .167e-     .144e-     -.523e-

Trapped  -  Zone       .000e-     .400e-     -.760e-

Net                     .000e-     .544e-     -.246e-

(*)-  Energy  Transfer  Summary  -(*)

Fate                         Heat  Rate  (W)              Change  of  Heat  (W)

Initial           Final        Sensible        Latent      React

----                     ----------      ----------      ----------     ----------   -------

Evaporated              -.180e+      .000e+     -.382e+     .214e+     .

Escaped  -  Zone        .272e+      .519e+     -.487e+     .282e+     .

Trapped  -  Zone        .954e+      .993e+     -.173e+     .051e+     .

----                     ----------      ----------      ----------     ----------    ------

Net                      .908e+      .351e+     -.998e+     .654e+     .

(*)-  Combusting  Particles  -(*)

Fate                Volatile  Content  (kg/s)             Char  Content  (kg/s)

Initial          Final      %Conv      Initial         Final

----                     ----------     ----------    -------   ----------    ----------

Evaporated               .000e+     .000e+       . .000e+    .000e+

Escaped  -  Zone        .333e-     .333e-       . .133e-    .133e-

Trapped  -  Zone        .333e-     .485e-     . .133e-    .133e-

Net                      .867e-     .333e-      . .267e-    .267e-

(*)  -  Multicomponent  Droplet  -(*)

Fate                            Species             Species  Content  (kg/s)

Names          Initial          Final       %Conv

----                            -------       ----------     ----------     -------

Evaporated              c5h12-droplet<l>      .667e-     .000e+      .

Evaporated              c7h16-droplet<l>      .333e-     .000e+      .

Evaporated                        h2o<l>      .000e+     .000e+        .

Escaped  -  Zone       c5h12-droplet<l>      .667e-     .585e-       .

Escaped  -  Zone       c7h16-droplet<l>      .000e+     .000e+        .

Escaped  -  Zone                 h2o<l>      .333e-     .134e-       .

Trapped  -  Zone       c5h12-droplet<l>      .333e-     .000e+      .

Trapped  -  Zone       c7h16-droplet<l>      .333e-     .000e+      .

Trapped  -  Zone                 h2o<l>      .333e-     .000e+      .

The report groups together particles with each possible fate, and reports the number of particles, the

time elapsed during trajectories, and the mass and energy transfer This information can be very

useful for obtaining information such as where particles are escaping from the domain, where particles

are colliding with surfaces, and the extent of heat and mass transfer to/from the particles within the

domain. Additional information is reported for combusting particles and multicomponent particles.

..... Elapsed Time

The number of particles with each fate is listed under the Number heading. (Particles that escape

through different zones or are trapped at different zones are considered to have different fates, and

are therefore listed separately.) The minimum, maximum, and average time elapsed during the tra-

jectories of these particles, as well as the standard deviation about the average time, are listed in

the Min, Max, Avg, and Std Dev columns. This information indicates how much time the particle(s)

spent in the domain before they escaped, aborted, evaporated, or were trapped.

Fate          Number                           Elapsed  Time  (s)

Min           Max            Avg       Std  Dev

----               ------      ----------     ----------    ----------      ----------   ---

Incomplete                     .485e+      .410e+     .947e+       .623e+

Escaped  -  Zone              .940e+      .196e+     .226e+       .871e+

Also, on the right side of the report are listed the injection name and index of the trajectories with

the minimum and maximum elapsed times. (You may need to use the scroll bar to view this inform-

ation.)

Elapsed  Time  (s)                                Injection,  Index

Min            Max           Avg      Std  Dev                     Min                 Max

---     ----------    ----------    ----------    --------------------  ------------------

+      .410e+     .947e+     .623e+        injection-        injection-

+      .196e+     .226e+     .871e+        injection-        injection-

..... Mass Transfer Summary

For all droplet or combusting particles with each fate, the total initial and final mass flow rates and

the change in mass flow rate are reported in the Initial, Final, and Change columns. With this

information, you can determine how much mass was transferred to the continuous phase from the

particles.

For unsteady tracking, the report lists the time-integrated mass flow rate of the particle streams that

have reached a particular fate at the current flow time. In other words, the report does not include

particles that are still being tracked in the domain.

Initial          Final         Change

----                  ----------     ----------     ----------

Incomplete             .388e-      .943e-      .194e-

Escaped  -  Zone      .502e-      .481e-     -.254e-

..... Energy Transfer Summary

This report tells you how much heat was transferred from the particles to the continuous phase. The

report is organized in two sections. For steady simulations, there is a Heat Rate and a Change

of Heat section. For unsteady particle tracking, there is an Energy and a Change of Energy

section. The Heat Rate and Energy sections are the same for all particle types, while the other

sections report the change of heat due to the various transfer processes, which differ for each particle

type. For steady simulations, the report lists the rate and the change of heat for the particle streams

organized according to the particle stream fates. For unsteady tracking, the report lists the time in-

tegrated heat rate and change of the particle streams that have reached a particular fate at the

current flow time. Note that the report does not include particles that are still being tracked in the

domain.

..... Heat Rate and Energy Reporting

domain.

For all particles with each fate, the total initial and final heat content are reported in the Initial

and Final columns. The particle heat content

is defined as follows:

Inert Particles:

(.)

where:

= mass flow rate of particles (kg/s)

= temperature of particles (K)

= heat capacity of particles (J/kg/K)

= reference temperature for enthalpy (K)

Droplet Particles:

(.)

where:

= heat of pyrolysis (J/kg)

= latent heat of evaporation at reference conditions (J/kg)

The latent heat at the reference conditions

is defined in Equation . in the Theory Guide.

Combusting Particles:

(.)

is the heat content of the evaporating/boiling liquid material if Wet Combustion is selected

(otherwise

= ).

(.)

where:

is the mass fraction of the liquid in the combusting particle

,

, and

are properties of the evaporating liquid material

is the heat content of the dry combusting particle and is calculated as

(.)

where:

is the volatile fraction

is the combustible fraction

Important

The Heat Rate section of the report is not provided for the multiple surface reactions

model.

Multicomponent Particles:

(.)

where:

= mass fraction of component i in particle

= heat content of component i

and

(.)

where:

= heat of pyrolysis for component i (J/kg)

= latent heat of evaporation at reference conditions for component i (J/kg)

= specific heat of component i (J/kg/K)

...... Change of Heat and Change of Energy Reporting

This section reports the total heat transferred from the particle to the continuous phase and is ana-

lyzed in components of Sensible heat, Latent heat and heat of Reaction. The Total change

reported equals the difference between the Initial and Final states of the particle streams.

The sensible heat component is reported for all particle types, the latent heat for the droplet, com-

busting and multicomponent particle, while the heat of reaction is reported for the combusting

particle type only. A positive Change of Heat denotes that heat is expelled from the continuous

phase and absorbed by the particle, while a negative Change of Heat denotes heat is released

by the particle to the continuous phase.

Steady and Transient Simulations

For steady simulations the report lists the heat rate

, while for unsteady tracking the time integrated

energy

from time  to current flow time

is reported.

(.)

Below is an example of an Energy Transfer Summary report for evaporating droplets:

Fate                    Heat  Rate  (W)           Change  of  Heat  (W)

Initial         Final       Sensible       Latent        Total

----               ----------    ----------     ----------   ----------   ----------

Evaporated        -.530e+    .000e+    -.750e+   .577e+   .530e+

Escaped-Zone     -.723e+   -.670e+    -.552e+   .282e+   .256e+

Trapped-Zone     -.176e+    .000e+    -.058e+   .187e+   .176e+

Net               -.353e+   -.670e+    -.085e+   .927e+   .886e+

Below is an example of an Energy Transfer Summary report for combusting particles:

Fate                 Heat  Rate  (W)             Change  of  Heat  (W)

Initial         Final      Sensible        Latent       Reaction      Tot

----             ----------    ----------    ----------    ----------     ----------   ------

Escaped-Zone      .697e+    .555e+    .166e+    .034e+    -.473e+    -.

Trapped-Zone      .886e+    .938e+    .731e+    .149e-    -.370e+     .

Net              .886e+    .493e+    .739e+    .149e+    -.474e+    -.

Important

In a coupled calculation, for all types of steady flows, the Total Net Change of

Heat reported in the Energy Transfer Summary should balance with the opposite

of the Sum over all fluid cells of the DPM Sensible Enthalpy Source. If this is not

the case, this means that the coupled discrete-continuous phase calculation has not

converged, and more DPM phase iterations are required. For more information on coupled

calculations, see Performing Trajectory Calculations (p. ).

Sum

DPM  Sensible  Enthalpy  Source                        (w)

--------------------------------       --------------------

fluid-                 -.

..... Combusting Particles

If combusting particles are present, ANSYS Fluent will include additional reporting on the volatiles

and char converted. These reports are intended to help you identify the composition of the combust-

ing particles as they exit the computational domain.

Fate                  Volatile  Content  (kg/s)           Char  Content  (kg/s)

Initial          Final     %Conv       Initial        Final     %Conv

----                   ----------     ----------   -------    ----------    ---------   -------

Incomplete              .247e-      .000e+    . .691e-    .000e+    .

Escaped  -  Zone       .758e-      .000e+    . .158e-    .782e-     .

The total volatile content at the start and end of the trajectory is reported in the Initial and

Final columns under Volatile Content. The percentage of volatiles that has been devolatilized

is reported in the %Conv column.

The total reactive portion (char) at the start and end of the trajectory is reported in the Initial

and Final columns under Char Content. The percentage of char that reacted is reported in the

%Conv column.

..... Combusting Particles with the Multiple Surface Reaction Model

If the multiple surface reaction model is used with combusting particles, ANSYS Fluent will include

additional reporting on the mass of the individual solid species that constitute the particle mass.

(*)-  Multiple  Surface  Reactions  -(*)

Fate                  Species       Species  Content  (kg/s)

Names       Initial        Final     %Conv

----                 -------    ----------   ----------   -------

Escaped  -  Zone       c<s>     .080e-    .487e-    .

Escaped  -  Zone       s<s>     .200e-    .077e-     .

Escaped  -  Zone        cao     .000e+    .153e-      .

Escaped  -  Zone      caso4     .000e+    .266e-      .

Escaped  -  Zone      caco3     .000e-    .260e-     .

The total mass of each solid species in the particles at the start and end of the trajectory is reported

in the Initial and Final columns, respectively. The percentage of each species that is reacted

is reported in the %Conv column. Note that for the solid reaction products (for example, if the mass

of a solid species has increased in the particle), the conversion is reported to be .

..... Multicomponent Particles

If your simulation includes multicomponent particles, ANSYS Fluent generates an additional report

for the particle components.

Fate                              Species            Species  Content  (kg/s)

Names        Initial         Final      %Conv

----                             -------     ----------    ----------    -------

Evaporated              c5h12-droplet<l>     .667e-    .000e+     .

Evaporated              c7h16-droplet<l>     .333e-    .000e+     .

Evaporated                        h2o<l>     .000e+    .000e+       .

Escaped  -  Zone       c5h12-droplet<l>     .667e-    .585e-      .

Escaped  -  Zone       c7h16-droplet<l>     .000e+    .000e+       .

Escaped  -  Zone                 h2o<l>     .333e-    .134e-      .

Trapped  -  Zone       c5h12-droplet<l>     .333e-    .000e+     .

Trapped  -  Zone       c7h16-droplet<l>     .333e-    .000e+     .

Trapped  -  Zone                 h2o<l>     .333e-    .000e+     .

At times, you may want to obtain a detailed, step-by-step report of the particle trajectory/trajectories.

Such reports can be obtained in alphanumeric format. This capability allows you to monitor the particle

position, velocity, temperature, or diameter as the trajectory proceeds.

The procedure for generating files containing step-by-step reports is listed below:

. Follow steps  and  in Displaying of Trajectories (p. ) for displaying trajectories.You may want to track

only one particle stream at a time, using the Track Single Particle Stream option.

. Select Step by Step as the Report Type.

Important

This option is only available for steady-state cases. For transient cases, see Reporting of

Current Positions for Unsteady Tracking (p. ).

. Select File as the Report to option. (The Track button will become the Write... button.)

. In the Significant Figures field, enter the number of significant figures to be used in the step-by-step

report.

. Click the Reporting Variables... button.

. Figure . : The Reporting Variables Dialog Box

. In the Reporting Variables dialog box (Figure . :The Reporting Variables Dialog Box (p. )), you can

change the variables in the report.The list under Variables in Report contains all variables currently re-

ported.The list under Particle Variables contains the particle variables that are available for you to select.

You can use the following buttons to modify the Variables in Report list:

Remove: Removes selected variables from that list.

Default Variables: Restores the default list.

Add Variable: Adds selections to the report using.

Add Color by: Adds the Color by variable to the list of Variables in Report, which is the only way to

get cell values or customized field functions into the report.

Important

Note that it is possible to select one variable in the Reporting Variables dialog box

and a variable from the Color by drop-down list in the Particle Tracks dialog box,

however, each variable is reported only once.

. Click the Write... button and specify a file name for the step-by-step report file in The Select File Dialog

Box (p. ).

A detailed report similar to the following example will be saved to the specified file before the traject-

ories are plotted. (You may also choose to print the report in the console by choosing Console as the

Report to option and clicking Display or Track, but the report is very long that it is unlikely to be of

use to you in that form.)

FILE  TYPE:

COLUMNS:

TITLE: TRACK  HISTORY

COLUMN  TYPE  VARIABLE                          (UNITS)

------  ----  --------                          -------

ParticleResidenceTime             (s)

ParticleXPosition                 (m)

ParticleYPosition                 (m)

ParticleZPosition                 (m)

ParticleXVelocity                 (m/s)

ParticleYVelocity                 (m/s)

ParticleZVelocity                 (m/s)

ParticleDiameter                  (m)

ParticleTemperature               (K)

ParticleDensity                   (kg/m3)

ParticleMass                      (kg)

---------------------------------------------

.00000e+   .00000e-   .00000e-   .00000e-   .00000e+   . . . .

.07087e-   .00000e-   .00000e-   .00000e-   .23339e+   . . . .

.51617e-   .00000e-   .00000e-   .00000e-   .04417e+   . . . .

. . . . . .

. . . . . .

. . . . . .

The default step-by-step report lists the position, velocity, diameter, temperature, density and mass

of the particle at selected time steps along the trajectory. In addition, the variable you have selected

in the Color by list is also included. If you choose Console as the Report to option, the variable names

are written as the header of each column. (You may need to use the scroll bar to view all variables in

this column.)

Time       X-Position   Y-Position   Z-Position    X-Velocity   Y-Velocity    Z-Veloc

.000e+  .000e-    .120e-    .000e+    .000e+     .000e+     .000e

.672e-  .168e-    .128e-    .000e+    .010e+     .988e+     .000e

.342e-  .337e-    .137e-    .000e+    .019e+     .977e+     .000e

.010e-  .508e-    .145e-    .000e+    .028e+     .965e+     .000e

.675e-  .680e-    .153e-    .000e+    .038e+     .954e+     .000e

.338e-  .854e-    .161e-    .000e+    .047e+     .942e+     .000e

. . . . . . .

. . . . . . .

. . . . . . .

If you change the reporting variables, only those selected will appear in the report. The particle time

is always reported in the first column. Note that it is possible to select one variable in the Reporting

Variables dialog box and a variable from the Color by drop-down list in the Particle Tracks dialog

box, however, each variable is reported only once.

When the report is written to a file, a table at the beginning of the file lists all variables selected with

the corresponding unit. Thus you can display or export any variable along a particle trajectory to the

console or to a file.

Note that the Coarsen option affects the step-by-step report.

In transient cases, when using unsteady tracking, you may want to obtain a report of the particle tra-

jectory/trajectories showing the current positions of the particles. Selecting Current Positions under

Report Type in the Particle Tracks Dialog Box (p. ) enables the display of the current positions of

the particles.

The procedure for generating files containing current position reports is listed below:

. Select Current Position as the Report Type.

. In the Significant Figures field, enter the number of significant figures to be used in the report.

Add Variable: Adds selections to the report.

Important

. Click the Write... button and specify a file name for the current position report file in The Select File Dialog

Box (p. ).

The default current position report lists the position, velocity, diameter, temperature, density, mass

and number in parcel of the particle at selected time steps along the trajectory. In addition, the variable

you have selected in the Color by list is also included. If you change the reporting variables, only those

selected will appear in the report. The particle time is always reported in the first column. It is possible

to select one variable in the Reporting Variables dialog box and a variable from the Color by drop-

down list in the Particle Tracks dialog box, however, each variable is reported only once.

The output to a file or to the console has the same format as the step-by-step report for steady-state

cases.

Time        X-Position    Y-Position    Z-Position   X-Velocity    Y-Velocity    Z-Velocity

.000e+     .000e-     .120e-     .000e+     .000e+     .000e+     .000e+

cases.

.672e-     .168e-     .128e-     .000e+     .010e+     .988e+     .000e+

.342e-     .337e-     .137e-     .000e+     .019e+     .977e+     .000e+

.010e-     .508e-     .145e-     .000e+     .028e+     .965e+     .000e+

.675e-     .680e-     .153e-     .000e+     .038e+     .954e+     .000e+

.338e-     .854e-     .161e-     .000e+     .047e+     .942e+     .000e+

. . . . . . .

. . . . . . .

. . . . . . .

Also listed are the diameter, temperature, density, mass of the particles, number in parcel and the

variable selected from the Color by list. (You may need to use the scroll bar to view this information.)

Time        Diameter   Temperature   Density        Mass          Number     ColorBy

.999e-     .352e-   .710e+   .840e+     .929e-     .792e+   .783e-

.999e-     .952e-   .710e+   .840e+     .801e-     .792e+   .834e-

.000e-     .660e-   .710e+   .840e+     .058e-     .792e+   .989e-

.001e-     .425e-   .710e+   .840e+     .719e-     .792e+   .719e-

.001e-     .184e-   .710e+   .840e+     .624e-     .792e+   .978e-

. . . . . . .

. . . . . . .

. . . . . . .

ANSYS Fluent reports the magnitudes of the interphase exchange of momentum, heat, and mass in

each control volume in your ANSYS Fluent model. You can display these variables graphically, by

drawing contours, profiles, and so on. They are all contained in the Discrete Phase Sources... category

of the variable selection drop-down list that appears in postprocessing dialog boxes:

DPM X,Y,Z Momentum Source

DPM Swirl Momentum Source

DPM Turbulent Kinetic Energy Source

DPM (species) Source

See Field Function Definitions (p. ) for definitions of these variables.

Note that these exchange terms are updated and displayed only when coupled calculations are per-

formed. Displaying and reporting particle trajectories (as described in Displaying of Trajectories (p. )

and Reporting of Trajectory Fates (p. )) will not affect the values of these exchange terms.

The exchange terms are reported as the rate occurring in each cell. A unit cell depth is used for 2D

cases, and a reference cell depth of  radian is used for 2D axisymmetric cases.

ANSYS Fluent reports various discrete phase particle/parcel quantities including erosion/accretion rates,

radiation quantities, and (optionally) cell-averaged particle size, velocity, temperature, and so on. You

can display these variables graphically, by drawing contours, profiles, and so on. They are accessed in

the Discrete Phase Variables... category of the variable selection drop-down list that appears in

Several quantities are automatically available depending on the models being used in the simulation.

For the cell-averaged quantities to be available, you must first enable Mean Values under Contour

Plots for DPM Variables in the Discrete Phase Model dialog box, Discrete Phase Model Dialog

Box (p. ). RMS quantities are also available for particle velocity and temperature by enabling RMS

Values.

Note

Enabling Mean Values to track the cell-averaged variables will increase the memory

requirements of your simulation.

The following lists specify those variables that are available automatically and those that require you

to enable them

Variables available automatically

DPM Erosion Rate (Generic)

DPM Erosion Rate (Finnie)

DPM Erosion Rate (McLaury)

DPM Erosion Rate (Oka)

DPM Erosion Rate (Wall Shear)

DPM Wall X Force

DPM Wall Y Force

DPM Wall Z Force

DPM (species) Concentration

Particle rotation variables (Particle rotation simulations only)

Angular X Velocity

Angular Y Velocity

Angular Z Velocity

Angular Velocity Magnitude

Angular Velocity (in the Particle Vector Style dialog box)

Cell-averaged variables available when Mean Values are enabled

DPM Particles in Cell

DPM Parcels in Cell

DPM X,Y, Z Velocity

DPM Diameter

DPM Density

DPM Temperature

DPM Specific Heat

DPM D20

DPM D30

DPM D32

DPM D43

DPM Granular Temperature

DPM Conc. of (component)

RMS variables available when Mean Values and RMS Values are enabled

DPM RMS X,Y, Z Velocity

DPM RMS Temperature

DPM RMS Diameter

Note that these variables are updated and displayed only when coupled calculations are performed.

Displaying and reporting particle trajectories (as described in Displaying of Trajectories (p. ) and

Reporting of Trajectory Fates (p. )) will not affect the values of these variables.

Note

If you select Enable Node Based Averaging in the Numerics tab of the Discrete Phase

Model dialog box, any previously calculated DPM variables will be rendered useless and

need to be recomputed.

.... Note on the Cell-Averaging of Particle Variables

DPM particles are actually numerical parcels, each of which can represent an arbitrary number of

physical particles. Therefore, a parcel representing many physical particles contributes more to the

averaging in a cell it crosses than a parcel representing fewer physical particles.

Likewise, a parcel that spends more time in a cell contributes more to the averaging in that cell than

a parcel that leaves the cell very soon after entering it (for example, when it passes only through a

corner of the cell, very close to the node).

These important aspects of weighting are accounted for in the calculation of the DPM variables that

are available as postprocessing cell-wise field variables in ANSYS Fluent.

If you are performing a transient simulation, you can include the computation of unsteady time stat-

istics (mean and RMS) for the discrete phase(s) of the transient flow. These are computed on a per-

phase basis by event-based time averaging over the discrete phase parcels in the domain. This means

that the sampling of the discrete phase particle quantity in a given cell occurs when (and only when)

a parcel passes through the cell.

To calculate the unsteady DPM time statistics, enable Data Sampling for Time Statistics in the Run

Calculation task page and enable DPM Variables in the Sampling Options dialog box when preparing

to run your simulation (see User Inputs for Time-Dependent Problems (p. )).

For a discrete phase variable,

, the event-based time average (mean) in a cell is calculated from

(.)

where

is the number of parcels in the domain, and

(.)

Here

is the number of particles in the

th parcel and  is the residence time of the

th parcel in

the cell. The weighting by residence time is necessary because a parcel may pass through more than

one cell within a computational time step and therefore its contribution to the averaged cell quantities

depends on the fraction of the time step spent in each cell.

The time-averaged DPM volume fraction is calculated from the individual number of particles in the

parcel, the particle volume, and its residence time in the cell in relation to the individual time step.

The RMS value is also available and is computed from Equation . (p. ).

(.)

Note that these quantities are averaged over all parcels that have passed through the cell and are

therefore different from the instantaneous cell-averaged values described in Reporting of Discrete

Phase Variables (p. ).

If you are using Data Sampling for Time Statistics, the same weighting is applied in the Unsteady

DPM Statistics... category as described in Note on the Cell-Averaging of Particle Variables (p. ). That

means that in the averaging over time steps, the phase velocity in the cell for a time step in which

many parcels spend a long time in that cell is given a larger weight than for a time step in which

fewer parcels spend less time in the same cell.

Below is a list of the available unsteady statistics when DPM Variables is enabled in the Sampling

Options dialog box. These are accessible by selecting the Unsteady DPM Statistics... category in

postprocessing or reporting dialog boxes. Note that the availability of some quantities depends on

the physics models being used. For definitions of these quantities, refer to the definitions of the in-

stantaneous quantities from which they are derived (see Alphabetical Listing of Field Variables and

Their Definitions (p. )).

Unsteady DPM Statistics

Mean DPM Volume Fraction

Accum DPM Particles in Cell

Mean DPM X,Y, Z Velocity

Mean DPM Diameter

Mean DPM Density

Mean DPM Temperature

Mean DPM Granular Temperature

Mean DPM Number Density

Accum DPM Parcels in Cell

Mean DPM D20

Mean DPM D30

Mean DPM D32

Mean DPM D43

RMS DPM Volume Fraction

RMS DPM X,Y, Z Velocity

RMS DPM Diameter

RMS DPM Density

RMS DPM Temperature

RMS DPM Granular Temperature

RMS DPM Number Density

Explanations for the Accum... variables are provided in Alphabetical Listing of Field Variables and Their

Definitions (p. ).

Particle states (position, velocity, diameter, temperature, and mass flow rate) can be written to files at

various boundaries and planes (lines in 2D) using the Sample Trajectories Dialog Box (p. ) (Fig-

ure . : The Sample Trajectories Dialog Box (p. )).

Results → Reports → Discrete Phase → Sample

Edit...

Figure . : The Sample Trajectories Dialog Box

The procedure for generating files containing the particle samples is listed below:

. Select the injections to be tracked in the Release From Injections list.

. Select the surfaces at which samples will be written These can be boundaries from the Boundaries list

or planes from the Planes list (in 3D) or lines from the Lines list (in 2D).

. If you want to use the particle sampling file as an unsteady injection file, select Sort Sample Files.

The Sort Sample Files option causes the sample files to be sorted in a reproducible manner. For

steady particle tracking, files will be sorted first by injection and then by particle ID. For unsteady

particle tracking, the files will be sorted strictly by the simulated time (flow-time in the 13th

column in the sample file) at which the particle passes the sampling plane surface or mesh zone.

. Click the Compute button. Note that for unsteady particle tracking, the Compute button will become

the Start button (to initiate sampling) or a Stop button (to stop sampling).

Clicking the Compute button will cause the particles to be tracked and their status to be written to

files when they encounter selected surfaces. The file names will be formed by appending .dpm to the

surface name.

Note

If you select a face zone in a mesh interface for sampling, Fluent will sample the particles

on both of the interface zones and will write out a total of three files. Two of these

files correspond to the particles that encounter each respective interface zone from

upstream. The third file contains the complete set of particles that have crossed the

mesh interface pair (via either interface zone).

For unsteady particle tracking, clicking the Start button will open the files and write the file header

sections. If the solution is advanced in time by computing some time steps, the particle trajectories

will be updated and the particle states will be written to the files as they cross the selected planes or

boundaries. Clicking the Stop button will close the files and end the sampling.

For stochastic tracking, it may be useful to repeat this process multiple times and append the results

to the same file, while monitoring the sample statistics at each update. To do this, enable the Append

Files option before repeating the calculation (clicking Compute). Similarly, you can cause erosion and

accretion rates to be accumulated for repeated trajectory calculations by turning on the Accumulate

Erosion/Accretion Rates option. (See also Postprocessing of Erosion/Accretion Rates (p. ).)

The format and the information written for the sample output can also be controlled through a user-

defined function, which can be selected in the Output drop-down list. More information about user-

The generated sample files can be used as injection file in a file injection. Both files use the same file

formats which differ between steady and unsteady particle tracking. For details, see Point Properties

for File Injections (p. ).

If the number of lines in the sampling file is large, you can reduce it by combining sets of similar line

entries into one single entry per such set. The mass represented by that entry will be increased accord-

ingly to ensure mass conservation. For details, see Data Reduction of Samples (p. ).

DPM sample files can be created using the Sample Trajectories Dialog Box (p. ) (as described in

Sampling of Trajectories (p. )) or by the VOF-to-DPM model transition mechanism. Such a file contains

multiple records, each consisting of values for the same set of variables. You can postprocess probab-

ility distributions and simple correlation analyses of these variables using the Trajectory Sample Histo-

grams Dialog Box (p. ) (Figure . : The Trajectory Sample Histograms Dialog Box (p. )).

Results → Reports → Discrete Phase → Histogram

Edit...

Figure . : The Trajectory Sample Histograms Dialog Box

.... Analysis, Investigation, and Reporting of Samples

The basic procedure for plotting a histogram of the probability distribution of a variable read from

data in a sample file is listed below:

. Select a sample file to be read by clicking the Read... button. After you read in the sample file, the sample

name will appear in the Sample list.

. Select the data sample in the Sample list, and then select the variable for which to plot the probability

distribution histogram from the Variable list.

. Select the variable by which to weight the file individual line entries from the Weight list.To obtain

representative information for most intensive variables, such as temperature, velocity, or position, you

should select:

mass-flow for a sample file from steady-state particle tracking

parcel-mass for a sample file from unsteady particle-tracking.

If the sampled particle streams / parcels all have the same flow rate / parcel mass, you can clear

Weighting.

. You can specify the number of bins, or intervals, in the plot in the Divisions field under Histogram

Parameters.

. If you want to plot just some part of the probability distribution, clear Auto Range and specify the range

of values in the Min and Max fields under Histogram Parameters.You can reset Min and Max to the

complete range by clicking Compute.

. If variable values you are investigating span several orders of magnitude, you can use logarithmic scaling

of the bins by selecting Logarithmic under Histogram Options. Note that this option is available only

for the variables that take only positive values.With this option, you should select the logarithmic scaling

format for the abscissa and, if necessary, for the ordinate in the Axes dialog box that opens by clicking

Axes… (Histogram Parameters group box).

. Click the Plot button at the bottom of the dialog box to display the histogram in the graphics window.

By default, the percentages of the total amount measured by the weighting variable will be plotted

on the  axis. You can plot the actual number of sampled particle streams / parcels (that is, line

entries from the file that fall into each interval on the  axis) by clearing Percent under Histogram

Options. If Weighting is selected, the sum of the weights of all entries in each bin will be plotted

instead of the number.

To display a probability density function curve instead of the histogram, clear Histogram Mode under

Histogram Options. You can enable the display of data point markers in the plot using the Curves

dialog box that opens by clicking Curve....

If you want to display in the console a summary for the selected variables similar to that in Summary

Reporting of Current Particles (p. ), select Diameter Statistics and click Plot. Although these stat-

istics are computed for any selected variable in the Variable list, it is applicable only to the diameter

If you want to further postprocess the plot data with other software tools, you can store them in an

XY-plot file format using the Write... button. If you use the default filename extension .his, the file

be written with a header. The header lines begin with the comment character ; and contain the same

statistical information that is printed to the Fluent console when you click Plot.

If you want to remove the currently highlighted sample from the Sample list and delete it from the

ANSYS Fluent session memory, but not the corresponding file, click Delete.

When investigating the behavior of particles, it is sometimes desirable to know how one particle

variable correlates with another particle variable. To facilitate this, the Correlation option exists. When

you enable this option, an additional column of sampled variables appears, allowing you to choose

the correlation variable (see Figure . : The Trajectory Sample Histograms Dialog Box: Correla-

tion (p. )). In this mode, every ordinate value will be a weighted average of the values of the cor-

relation variable in all entries that fall into the respective bin.

Figure . : The Trajectory Sample Histograms Dialog Box: Correlation

If you want to plot the continuous cumulative distribution function, enable the Cumulative Curve

option. A cumulative distribution curve is computed of the variable that is selected in the Variable

list using the weighting options. However, if the Correlation option is enabled along with the Cumu-

lative Curve, then the cumulative curve of the variable selected in the Correlation list is plotted. For

a constant particle density, you can plot a correlation curve for the particle mass by selecting the

diameter as a Correlation variable and enabling (Variable)ˆ3. This calculates cubes of the variable

chosen under Correlation and for which an average is calculated within each bin and used for the

ordinate value in the plot as explained above.

.... Data Reduction of Samples

When you use a sample file as an injection file in a subsequent simulation, it may be desirable to reduce

the number of particles injected by the file in order to lower the computational cost. In ANSYS Fluent

this can be done by reducing the number of lines the sample file contains using a method that is

similar to that used to create a histogram. However, unlike a histogram, the weighted entries from

the sample file are sorted into intervals for all variables simultaneously, not one variable at a time.

The method first sorts all file entries into groups, or bins, of entries that are sufficiently similar in all

properties. The entries that have fallen into the same bin are then averaged to create a single entry.

Conservation of mass and volume as well as the number of particles is achieved by appropriate

weighting in the averaging process.

To reduce a sample file size:

. Read a sample file as described in Analysis, Investigation, and Reporting of Samples (p. ).

. Select the data sample in the Sample list.

. Select Data File Reduction.

The Trajectory Sample Histograms dialog box will expand to show the Scale, No. of Bins list

(between the Variable and Weight lists) and data file reduction inputs.

Figure . : The Trajectory Sample Histograms Dialog Box: Data File Reduction

. For each variable in the Variable list, specify the following parameters in the Data Reduction in the

Selected Variable group box:

1st Bin Min , Last Bin Max

limit the range of values to consider. Note that the complete range for the selected variable is displayed

in the Min and Max fields in the Histogram Parameters group box.You can use the Reset button

to reset 1st Bin Min and Last Bin Max to their original values.

LOG Scale

enables the use of a logarithmic scale.The behavior of this option is analogous to the Logarithmic

option in Histogram Options (see Analysis, Investigation, and Reporting of Samples (p. )). By de-

fault, the linear scaling is used.This option is available only if all values for the variable in the sample

file are positive.

No. of Bins

No. of Bins

the number of groups into which the specified range for this variable is to be divided. If you want

to neglect any variable, set No. of Bins to . If you want to set the value you specified for all variables,

click Set No. of Bins for All Variable.

Once you have specified 1st Bin Min, Last Bin Max, and No. of Bins, you can click Update to

see the Resulting Bin Size. If the LOG Scale is selected, the value shown in the Resulting Bin

Size is the ratio for LOG Scale.

You can quickly review the inputs for the scaling and number of bins for each variable in the

Scale, No. of Bins information list.

. For a standard DPM sample file generated by ANSYS Fluent, you should use the default weighting.

However, if you want to reduce data in a file that does not contain the default header and variable

columns that are present in a standard DPM sample file, you can select a weighting variable manually

from the Weight list. If you do not want to use the weight, clear the Weighting option in the Data Re-

duction Options group box. Note that in both scenarios, the reduced sample file may not represent the

same mass, volume, and flow rates of discrete phase.

. If the original sample file was generated from unsteady particle tracking, you can reduce the unsteady

sample file to a regular steady-state injection file by selecting the Create Steady from Unsteady check

box in the Data Reduction Options group box.This option is available only for sample files from unsteady

particle tracking.

. Once you have configured the data reduction settings for all variables and selected the data reduction

options, click Reduce....

. In The Select File Dialog Box (p. ) that opens automatically, enter the name of your reduced injection

sample file.

The number of aggregated records will be reported in the ANSYS Fluent console.

For many mass-transfer and flow processes, it is desirable to know the mean diameter of the particles.

A mean diameter,

, is calculated from the particle size distribution using the following general ex-

pression  [] (p. ):

(.)

where  and  are integers and

is the distribution function (for example, Rosin-Rammler).

,

for example, is the average (arithmetic) particle diameter. The Sauter mean diameter (SMD),

, is the

diameter of a particle whose ratio of volume to surface area is equal to that of all particles in the

computation. A summary of common mean diameters is given in Table . : Common Mean Diameters

and Their Fields of Application (p. ).

Table . : Common Mean Diameters and Their Fields of Application

Field of Application

Name

Order

Comparisons, evaporation

Mean diameter,

Absorption

Mean surface diameter,

Hydrology

Mean volume diameter,

Name

Order

Adsorption

Overall surface diameter,

Evaporation, molecular diffusion

Overall volume diameter,

Combustion, mass transfer, and

efficiency studies

Sauter mean diameter,

Combustion equilibrium

De Brouckere diameter,

Summary information (number, mass, average diameter) for particles currently in the computational

domain can be reported using the Particle Summary Dialog Box (p. ) (Figure . : The Particle

Summary Dialog Box (p. ))

Results → Reports → Discrete Phase → Summary

Edit...

Figure . : The Particle Summary Dialog Box

The procedure for reporting a summary for particle injections is as follows:

. Select the particle injection(s) you want summarized in the Injections list.

Fluent provides a shortcut for selecting injections with names that match a specified pattern. To

use this shortcut, enter the pattern in the Filter Text box. For example, if you specify drop*, all

injections that have names beginning with drop (for example, drop-, droplet) will be listed.

. Click Summary to display the injection summary in the console window.

(*)-  Summary  for  Injection:  injection-  -(*)

Total  number  of  parcels              :

Total  number  of  particles            :  .196710e+

Total  mass                             :  .128303e- (kg)

Maximum  RMS  distance  from  injector  :  .372527e- (m)

Maximum  particle  diameter             :  .072739e- (m)

Minimum  particle  diameter             :  .756993e- (m)

Overall  RR  Spread  Parameter          :  .446806e+

Maximum  Error  in  RR  fit             :  .071220e-

Overall  RR  diameter             (D_RR):  .051303e- (m)

Overall  mean  diameter           (D_10):  .663269e- (m)

Overall  mean  surface  area      (D_20):  .344694e- (m)

Overall  mean  volume             (D_30):  .121478e- (m)

Overall  surface  diameter        (D_21):  .125692e- (m)

Overall  volume  diameter         (D_31):  .013570e- (m)

Overall  Sauter  diameter         (D_32):  .030141e- (m)

Overall  De  Brouckere  diameter  (D_43):  .082971e- (m)

You can calculate the erosion and accretion rates in a cumulative manner (over a series of injections)

by using the Sample Trajectories dialog box. First select an injection in the Release From Injections

list and compute its trajectory. Then enable the Accumulate Erosion/Accretion Rates option, select

the next injection (after deselecting the first one), and click Compute again. The rates will accumulate

at the surfaces each time you click Compute.

Important

Both the erosion rate and the accretion rate are defined at wall face surfaces only, so they

cannot be displayed at node values.

... Assessing the Risk for Solids Deposit Formation During Selective

Catalytic Reduction Process

ANSYS Fluent provides functionality for assessing the solids deposition risk in the Selective Catalytic

Reduction (SCR) process. The computation involves several chemical and hydrodynamic risk factors

that are based on thermodynamic data and known chemical pathways, as well as on experimental

evidence reported in the literature ([] (p. ), [] (p. ), [] (p. ), [] (p. ), and

[] (p. )). The risk assessment calculation should be invoked after the initial liquid film formation

on the surfaces of the SCR device, and should cover a time period over one or more urea injection

cycles. The risk variables are defined as dimensionless quantities that vary from  to , where  corres-

ponds to no risk and  corresponds to maximum risk. Note that the risk assessment calculation is not

a predictive model for urea deposit formation, and the obtained results should be considered only as

rough guidance in exploring urea deposit formation trends.

The implementation takes into account the following chemistry risk factors:

Crystallization risk

The limiting urea mass fraction

for the onset of crystallization is a function of film temper-

ature

([] (p. ) and [] (p. )). Therefore, the crystallization risk over the time

period

–

can be calculated as the fraction of time when the urea mass fraction in the liquid

film

exceeds

:

(.)

Secondary reactions risk

According to [] (p. ), [] (p. ), and [] (p. ), the formation of biuret and/or cyanuric

acid solids deposits starts at

= - K and diminishes at

=  K. In addition, the

presence of HNCO in the gas phase above the film is required. It follows that the secondary

reactions risk over the time period

–

can be calculated as the fraction of time when the liquid

film is exposed to a non-zero HNCO concentration and the film temperature is between

and

as specified above.

(.)

In addition, the following hydrodynamic factors have been shown to affect solids deposit formation

trends:

Intense dynamics can be quantified as fluctuations of film height [] (p. ).When the fluctuations are

high, the risk of deposit formation is impeded.

As reported by Smith et al. [] (p. ), thick film and high film velocity indicates low deposit formation

risk, while Brack et al. [] (p. ) report that thick film and low heat flux indicate high deposit formation

risk.

Accordingly, ANSYS Fluent uses the following definitions to quantify the hydrodynamic risk factors:

Velocity-based risk

(.)

Heat-flux based risk

(.)

where

= (Wall Film Height) / (Maximum Film Height)

(.)

(.)

where

=(Wall Film Velocity) / (Maximum Wall Film Velocity)

= (Wall Film Heat Flux) / (Maximum Wall Film Heat Flux)

Finally, averaging over the period from

to

and applying appropriate weighting factors, the total

risk

is calculated as:

(.)

where:

(.)

(.)

The weighting factors

.

,

, and

are user-specified values.

You can access the functionality for assessing the risk of solids deposit formation via the following

text commands:

define/models/dpm/options/scr-urea-deposition-risk-analysis/enable? yes

You will be asked to define the wall zones where the risk assessment should be performed, for example:

Wall face zones() [()]

The implementation uses the data sampling and custom field functions in ANSYS Fluent, and after

enabling the risk assessment capability, the following steps are automatically performed:

Defining appropriate solution report definitions for calculating the maximum film height, velocity, and

heat-flux.

Defining the required custom field functions for calculating the risk factors.

Enabling data sampling on the custom field functions.

Once the SCR urea deposition risk analysis is enabled, you can set the following parameters and

weighting factors (available under define/models/dpm/options/scr-urea-deposition-

risk-analysis/):

cryst-min-temp and cryst-max-temp: the minimum and maximum film temperatures for the onset

of urea crystallization (K), respectively

cryst-min-mass-fract: the minimum urea mass fraction for the onset of urea crystallization as defined

in [] (p. ) and [] (p. )

seco-rx-min-hnco: the minimum HNCO mass fraction in the gas phase above the liquid film for sec-

ondary reactions (

in Equation . (p. ))

seco-rx-min-temp and seco-rx-max-temp: the minimum and maximum film temperatures for

secondary reactions (K), respectively (

and

hydrodynamic-risk-weight: weighting factor for hydrodynamic risk (

cryst-depo-weight: weighting factor for crystallization risk (

velocity-based-risk-weight: weighting factor for velocity based risk (

heat-flux-based-risk-weight: weighting factor for heat-flux based risk (

in Equa-

tion . (p. ))

wall-face-zones: wall zone list for solids deposit risk prediction

After the time-dependent calculation is completed, the following variables will be available under

Custom Field Functions... category for post-processing:

scr-urea-overall-hydrodynamic-deposition-risk: is

scr-urea-overall-chemistry-deposition-risk: is

scr-urea-total-deposition-risk:

Additional field variables reported under the Custom Filed Functions... and SCR Urea Deposition

Risk Analysis... categories are the following:

scr-urea-depo-risk-velocity-based (in the Custom Filed Functions... category):

scr-urea-depo-risk-heat-flux-based (in the Custom Filed Functions... category):

in Equa-

tion . (p. )

SCR Urea Crystallization Risk (in the SCR Urea Deposition Risk Analysis... category): is the chemistry

based risk representation

SCR Urea Secondary Reactions Risk (in the SCR Urea Deposition Risk Analysis... category): is the

chemistry based risk representation

SCR Overall Urea Chemical Deposition Risk (in the SCR Urea Deposition Risk Analysis... category): is

the chemistry based risk representation

You may ignore the additional variables with the scr-urea-depo- prefix in the Custom Filed Functions...

category as they are intermediate quantities with no meaningful values.

ANSYS Fluent offers three modes of parallel processing for the discrete phase model:

Shared Memory

The Shared Memory method is suitable for computations where the machine running the ANSYS

Fluent host process is an adequately large, shared-memory, multiprocessor machine.

Message Passing

The Message Passing option is suitable for generic distributed memory cluster computing.

Hybrid (default)

The Hybrid option is suitable for modern multicore memory cluster computing.

These options are found under the Parallel tab, in the Discrete Phase Model dialog box.

Important

models (VOF, mixture, or Eulerian) the Shared Memory method cannot be selected. (Note that

Starting in version ., the Shared Memory method is not compatible with serial UDFs when

running in serial.

If you want to use file injections or to write a DPM summary report directly to a file, your system must

meet the following requirements when either the Message Passing or Hybrid parallel DPM tracking

option is selected:

The machine (for example, cluster node) running the compute-node zero process and the machine running

the host process are identical or have the same operating system type (Windows or Linux)

Both machines can access the same file system through the same path specification

If these conditions are not met, you can still write a DPM summary report to a file by starting transcript,

reporting the particle tracking summary to the Fluent console, and then stopping transcript. The summary

report will be saved in the transcript file.

As a workaround for the DPM summary report, you can start transcript, report the particle tracking

summary to the Fluent console, and stop transcript. The summary report will be saved in the transcript

file

The Shared Memory option (Figure . : The Shared Memory Option with Workpile Algorithm En-

abled (p. )) is implemented using POSIX Threads (pthreads) based on a shared-memory model. Once

the Shared Memory option is enabled, you can then select along with it the Workpile Algorithm and

specify the Number of Threads. By default, the Number of Threads is equal to the number of compute

nodes specified for the parallel computation. You can modify this value based on the computational

requirements of the particle calculations. If, for example, the particle calculations require more compu-

tation than the flow calculation, you can increase the Number of Threads (up to the number of available

processors) to improve performance. When using the Shared Memory option, the particle calculations

are entirely managed by the ANSYS Fluent host process. You must make sure that the machine executing

the host process has enough memory to accommodate the entire mesh.

Important

Note that the Shared Memory option on Windows-based architectures only provides serial

tracking on the host, since the Workpile Algorithm is not available due to lack of POSIX

Threads on these platforms.

Important

Note that the Workpile Algorithm option is not available with the wall film boundary con-

dition. It will be disabled automatically when choosing to simulate a wall film on a wall.

Parallel Processing for the Discrete Phase Model

Figure . : The Shared Memory Option with Workpile Algorithm Enabled

The Message Passing option enables cluster computing and also works on shared-memory machines.

With this option enabled, the compute node processes perform the particle work on their local partitions.

Particle migration to other compute nodes is implemented using message passing primitives. There are

no special requirements for the host machine. Note that this model is not available if the Cloud Model

option is turned on under the Turbulent Dispersion tab of the Set Injection Properties dialog box.

By default, pathline displays are computed in serial on the host node. Pathline displays may be computed

in parallel on distributed memory systems if the Message Passing parallel option is selected in the

The Hybrid option combines Message Passing and OpenMP for a dynamic load balancing without

migration of cells, enables multicore cluster computing, and also works on shared-memory machines.

With this option enabled, the compute node processes perform the particle calculations on their local

partitions. OpenMP threads will be spawned, and the number of threads in each ANSYS Fluent node

process is based on the evaluation of the particle load on the current machine. The maximum number

of threads on each machine can be controlled using the Thread Control dialog box (see Controlling

the Threads (p. ) for details). The default value is the number of ANSYS Fluent node processes on

each machine. Particle migration to other compute nodes is implemented using message passing

primitives. There are no special requirements for the host machine. Note that this model is not available

if the Cloud Model option is turned on under the Turbulent Dispersion tab of the Set Injection

Properties dialog box. Pathline displays are computed by default in serial on the host node. Pathline

displays may also be computed in parallel on distributed memory systems if the Message Passing option

is selected from the Methods list. For a list of limitations that exist with Hybrid parallel method, see

Limitations on Using the Hybrid Parallel Method (p. ).

When using the Hybrid method, you may optionally enable Use DPM Domain under Hybrid Options.

This option can provide substantially improved load balancing, and thus scalability, at the expense of

additional memory overhead. When Use DPM Domain is enabled, particle tracking is performed on a

separate domain from the root computational domain. Flow and DPM variables are copied between

the domains as part of the solution process. By using a separate domain, and thus partitioning strategy,

for particle tracking the continuous and discrete phase loads are balanced independently. This allows

the load to be shared more equally among the machines regardless of how particles are distributed

throughout the computational domain. This is especially beneficial for simulations with non-uniform

particle distributions over the computational domain. For limitations associated with the Use DPM

Domain option, see Limitations on Using the Hybrid Parallel Method (p. ). With this option, you may

also want to use the following text commands:

parallel → partition → set → dpm-load-balancing

This text command enables dynamic load balancing. You will be prompted to define a load imbalance

threshold (that is, a percentage above which load balancing will occur), as well as the interval of DPM

iterations at which you would like load balancing attempted. It is recommended that you retain the

default values, as these are appropriate for a wide range of cases.

define → models → dpm → parallel → expert → partition-method-hybrid-2domain

This enables a partitioning method that is more granular and can yield faster calculations (especially

for cases that are running on a low to moderate number of processors).

You may seamlessly switch among the Shared Memory option, the Message Passing option, and the

Hybrid option at any time during the ANSYS Fluent session.

In addition to performing general parallel processing of the Discrete Phase Model, you have the option

of implementing DPM-specific user-defined functions in parallel ANSYS Fluent. For more information

about the parallelization of DPM UDFs, see Parallelization of Discrete Phase Model (DPM) UDFs in the

When using the Message Passing or the Hybrid option you can make use of ANSYS Fluent’s automated

load balancing capability by giving an appropriate weight to the particle steps in each cell. In this case

the number of particle steps in each partition is considered in the load balancing procedure. Further

details can be found in Using the Partitioning and Load Balancing Dialog Box (p. ).

Chapter : Modeling Macroscopic Particles

Traditional Lagrangian discrete phase models only apply when particle sizes are small enough to be

regarded as point masses within a single cell and when the total particle volume is insignificant within

the flow domain volume. In these applications particle-particle and particle-flow interactions are evaluated

in terms of impulse, heat, and mass transfer.

However, the total particle volume must be considered when a particle size is larger than several fluid

cells because it will affect all the cells within the flow domain volume. ANSYS Fluent Macroscopic Particle

Model (MPM) predicts the behavior of large (macroscopic) particles and their interaction with the fluid

flow, walls, and with other particles.

This chapter provides an overview of how to use the MPM add-on module in ANSYS Fluent. For more

information about the theoretical background for the MPM modeling approach, see Modeling Macro-

scopic Particles.

.. Overview and Limitations

.. Loading the MPM add-on Module

.. Setting up MPM Model Simulations

.. Modeling Macroscopic Particles

The MPM is an add-on module based on a suite of UDF functions that models transport of large particles

in a fluid flow, particle-particle and particle-wall interactions, as well as particle tracking. The MPM is

designed for macroscopic particles that are well-resolved across a particle diameter by at least -

fluid cells.

The MPM is not a general purpose model. The model has been shown to give good results for applications

in which macroscopic particles with Reynolds number

<<  move in a flow having a fluid-to-particle

density ratio,

, in the order of . For other values of

and

, the drag prediction may not

be accurate; in such cases the MPM model may be used when drag is not important.

Note the following limitations when using the MPM:

Mass transfer and radiation cannot be modeled.

The MPM is not compatible with moving/deforming meshes.

Simulations of densely-packed particles are not supported because only one collision event is handled for

each particle time step.

There is no direct interaction with DPM particles (collision).

Coupling with Multiphase models is possible, but manual settings are required for source terms (mass,

momentum, and heat).

Sub-iterations of MPM particle tracks within one time step are not supported.

The MPM is not compatible with mesh interfaces.

The MPM add-on module is installed with the standard installation of ANSYS Fluent in a directory called

addons/mpm. The MPM add-on module is loaded into ANSYS Fluent through the text user interface

(TUI). Note that the module can be loaded only when a valid ANSYS Fluent case file has been set or

read. To load the MPM add-on module, issue the following TUI command in the Fluent console:

define → models → addon-module

A list of ANSYS Fluent add-on modules is displayed in the console:

Fluent Addon Modules:

. none

. MHD Model

. Fiber Model

. Fuel Cell and Electrolysis Model

. SOFC Model with Unresolved Electrolyte

. Population Balance Model

. Adjoint Solver

. Single-Potential Battery Model

. Dual-Potential MSMD Battery Model

. PEM Fuel Cell Model

.Macroscopic Particle Model

Enter Module Number: []

Select the Macroscopic Particle Model by entering the module number . During the loading process,

a Scheme library containing the graphical and text user interface, and a UDF library containing a set of

user-defined functions (UDFs) for the MPM add-on module are automatically loaded into ANSYS Fluent.

This process is reported in the Fluent console. Once the MPM module is loaded into ANSYS Fluent, the

Macroscopic Particles model appears under the Models tree branch, and the UDF library also becomes

visible as a new entry in the UDF Library Manager dialog box. By default, the Macroscopic Particles

model is enabled.

Note

The MPM model is only available in 3D.

Note

The following procedure provides an overview of the steps required for setting up and solving an MPM

model case. Only the steps that are pertinent to MPM modeling are shown here. For information about

inputs related to other models that you want to use in conjunction with the MPM model, see the ap-

propriate sections for those models in the ANSYS Fluent User's Guide (p. ).

.

Use Fluent Launcher to start the 3D version of ANSYS Fluent.

.

Read the case or mesh file.

.

Scale the mesh, if necessary.

.

For most cases except for cemented particles simulations, select the Transient solver from the Time list

in the General task page.

Modeling Macroscopic Particles

.

Define the boundary conditions and physical properties for fluid flow as usual.

.

(optional) Initialize the flow variables and run the flow simulation until the flow converges.

This step could be performed to improve solution stability. Using a converged flow solution as a

starting point for an MPM simulation can be particularly helpful in situations where there is a strong

influence of macroscopic particles on the fluid flow.

.

Use the Macroscopic Particle Model dialog box to specify the parameters for the MPM simulation.

.

Initialize either the MPM model as described in the sections that follow or the flow field in the usual way.

.

Run the MPM simulation.

. Save the case and data files, if desired.

. Review the simulation results by generating plots or alphanumeric reports using the ANSYS Fluent post-

processing facilities.

You can set the MPM model parameters and select the options that are appropriate for your simulation

using the Macroscopic Particle Model dialog box that opens from the Setup/Models/Macroscopic

Particle tree item. From the Macroscopic Particle Model dialog box, you can access the Create/Modify

Injection dialog boxes, where you can set the macroscopic particle injection properties.

Setup → Models → Macroscopic Particle

Edit...

Figure . : Macroscopic Particle Model Dialog Box (Particle Tracking Tab)

The inputs for the MPM model are entered using the following tabs:

Particle Tracking

is where you can define parameters for particle tracking.

Drag

contains drag law options and parameters for the particle drag calculations.

Collision

allows you to enable particle-particle and particle-wall collisions and define the collision parameters.

Deposition

allows you to enable particle deposition on selected surfaces and particles and define the relevant para-

meters.

Injections

allows you to define macroscopic particle injections.

Attraction Forces

is where you can specify parameters for particle-particle and particle-wall attraction forces.

Initialize MPM

contains controls for initializing the macroscopic particles and displaying particle injections.

Note

The default settings may not be appropriate for your case. You must provide parameter data

for your specific material.

... Specifying Particle Tracking Parameters

... Specifying the Drag Law

... Defining Parameters for Particle-Particle and Particle-Wall Collisions

... Specifying Deposition Parameters

... Specifying Injection Parameters

... Defining Field Forces

... Initializing the MPM model

You can use the Particle Tracking tab to control the solution process of the MPM trajectory equations

using the following settings (see Figure . : Macroscopic Particle Model Dialog Box (Particle Tracking

Tab) (p. )):

Particle Zones

contains a selectable list of the cell zones in which you can use the MPM model.

Enable Interaction with Continuous Phase

(if selected) enables two-way coupling between particles and fluid flow.

Particle Sub-Timesteps within each Flow Timetep

is a number of sub-time steps for particle tracking in each flow time step.

Under-Relaxation Factor to Velocities in Touched Cells

By default the under-relaxation factor for fixing velocities is set to .

Solve Heat Transfer

enables solving the energy equation.When this option is enabled, you will need to specify Initial Tem-

perature and Specific Heat for a particle material in the Create/Modify Injection dialog box.

Note

The particle time step should be chosen so that macroscopic particles do not cross more

than one CFD mesh cell.

Under the Drag tab, you can select an appropriate drag law for your simulation and set the relevant

parameters or select Disable Drag Calculations if you do not want to model the drag force in the

domain.

Figure . : Macroscopic Particle Model Dialog Box (Drag Tab)

In the ANSYS Fluent MPM model, the following formulations are available for modeling the drag forces

domain.

between the continuous and macroscopic particle phases:

Momentum Deficit Rate (MDR) (default)

In this formulation, the momentum exchange coefficient between fluid and solid phases

is cal-

culated as:

where  is the drag function, and

is the macroscopic particle time step.

The accuracy of the implicit calculations using the Momentum Deficit Rate model depends on

number of cells comprising the macroscopic particle. This drag correlation is more suitable for bigger

size particles.

Morsi-Alexander (MA)

In the Morsi-Alexander based drag correlation  adopted in ANSYS Fluent, the Reynolds number

for the fluid phase is calculated by:

where,

= fluid viscosity

= particle diameter

= relative velocity of the discrete and fluid phases

The Morsi-Alexander based drag correlation is suitable for smaller size particles.

Constant Drag Coefficient (Cd)

This option implies that the drag is evaluated using a constant drag coefficient. This correlation is

suitable for cases where the particle is moving at a certain specified velocity (or acceleration).

Size Based MA/MDR

When this option is selected, the ANSYS Fluent solver automatically switches between the Momentum

Deficit Rate and Morsi-Alexander drag laws based on a critical diameter. This drag formulation is

best suited for cases involving wide range of particle sizes in a single simulation. For particles with

a diameter below the value that you specify for Critical Diameter, the Mosi-Alexander drag law will

be used. Otherwise, the Momentum Deficit Rate formulation will be used.

You can define a drag factor in a specific direction (X-dir,Y-dir,Z-dir). A drag factor of  means that

the virtual mass force equalizes the momentum difference of fluid in cells touched by the particle

surface within a single flow time step. As a consequence, the particle sub-time step has to be much

smaller (about one-fourth) than the momentum relaxation time

:

where

and

are the particle and fluid densities, respectively,

is the particle diameter, and  is

the fluid viscosity.

Besides, the accuracy of the predicted drag depends on the number of cells touched by the particle.

At least - cells are required across the particle diameter.

For multiphase flows, you can select an appropriate fluid velocity field to be used in the drag force

calculations. The following options are available in the Multiphase: Drag Based On group box:

Primary Phase Velocity

Secondary Phase Velocity

Volume-Weighted Mixture Velocity

The Collision tab allows you to model the effects of particle-particle and particle-wall collisions.

Figure . : Macroscopic Particle Model Dialog Box (Collision Tab)

To account for collisions between particles:

. Select Enable Particle-Particle Collision.

. Specify the following parameters:

Coefficient of Restitution (Normal Dir)

corresponds to

Coefficient of Restitution (Tangential Dir)

Substeps For Collision

is a number of sub-time steps for detecting particle collision in each particle tracking time step.

Coefficient of Friction

If you also want to account for collisions between particles and walls:

. Select Enable Particle-Wall Collision.

. From the Participating Zones For Collision selection list, select the appropriate walls.

. In addition to Coefficient of Restitution (Normal Dir) and Coefficient of Restitution (Tangential Dir)

on the selected walls, you can specify the following parameters:

Coefficient of Friction (Sliding)

Coefficient of Friction (Rolling)

The value for the rolling coefficient of friction will be factored in the friction coefficient

.

You can use the Deposition tab to specify parameters for macroscopic particle deposition and buildup

on selected zones.

Figure . : Macroscopic Particle Model Dialog Box (Deposition Tab)

. Select Enable Particle-Wall Deposition.

. From the Zones for Deposition selection list, select the wall zones on which the macroscopic particles

will adhere upon collision.

. Specify the following deposition parameters:

Minimum Drag Force for Particle Detachment

specifies the force at or above which the deposited particles detach from a surface zone.

Max Normal Velocity for Particle Deposition , Max Tangential Velocity for Particle Deposition

specify the normal and tangential components of the approach velocity at or below which the particles

deposit on the surface.

. If you want to save particle deposition history data in ASCII format, enable Write Particle Deposition

File.

File.

. To account for particle agglomeration, select Enable Particle-Particle Deposition. A particle that collides

with any previously deposited particles will attach to the particle surface.The deposition parameters that

you have specified for particle-wall deposition will be also used for modeling particle-particle deposition.

You can use the Injections tab to create, edit, copy or delete macroscopic particle injections. You can

also save all particle injections that you have created to a file for later use or read injections from a

previously generated file. The controls under the Injection tab are similar to those found in the Injec-

tions dialog box (see Injections Dialog Box in the Fluent User's Guide (p. )) with a few minor differ-

ences.

Figure . : Macroscopic Particle Model Dialog Box (Injection Tab)

The procedures for creating, modifying and interacting with injections are also similar to those for the

DPM injections. The differences related to the MPM injections will be further emphasized. For more

information about using these controls, see the Fluent User’s Guide.

To create an MPM injection: click Create... and set the injection properties using the Create/Modify Injection

dialog box (see Defining MPM Injection Properties (p. )). After the injection is created, it will appear in

the Injections selection list, in the Macroscopic Particle Model dialog box.

To edit an existing MPM injection: select it from the Injections selection list, click Edit..., and in the Cre-

ate/Modify Injection dialog box that will open, modify the injection properties as necessary .

To copy an existing MPM injection to a new injection: select it from the Injections selection list and click

Copy.The name of the new copied injection appended with _d will appear in the Injections list.

To delete an existing MPM injection: select it from the Injections selection list and click Delete.

To write information about all injections created in a case: click Write All Injections... and in the Select

File dialog box that will open, enter the name for the injection file.

Note

Write All Injections... is not supported for steady flows with cemented particles.

To read previously generated injection file into your case: click Read... and in the Select File dialog box

that will open, select the injection file to read in. If the injection with the same name already exists in your

current case, then ANSYS Fluent will rename the imported injection by appending _d to the name.

.... Defining MPM Injection Properties

You can define the properties of an MPM injection using the Create/Modify Injection dialog box

that can be accessed by clicking Create.... The procedure for defining a particle injection is as follows:

. (Optional) Change the default name of the injection (injection-id ) by entering a new name in the

Injection Name entry field.

. From the Injection Type drop-down list, select the injection type. In the ANSYS Fluent MPM model, you

can create the following types of injections:

point: defines an injection released from a single point.

plane: defines uniformly or randomly distributed injections released from a plane.

packing: defines an injection of particles packed in a box or cylinder.

from-file: allows you to read a text file that defines an injection.

. If you want to model fixed particles, enable Cemented Particle(s).

Important

For steady-state simulations, all particles must be cemented.

. Specify the particle physical parameters (Diameter and Density).

Note

Note that a material defined in ANSYS Fluent cannot be assigned to a particle.

. Specify the injection type-specific settings as described in the following sections:

point injections: Inputs for point Injections (p. )

plane injections: Inputs for plane Injections (p. )

packing injections: Inputs for packing Injections (p. )

from-file injections: Inputs for from-file Injections (p. )

. (Optional) If you want to model a continuous generation of particle injections, select Enable Continuous

Injection and in the Define Continuous Injection dialog box that opens when you click Set..., specify

the relevant parameters.

You can specify the following settings:

Injection start, stop, and interval times

New macroscopic particle will be injected into the domain at regular time intervals specified in

Injection Interval Time from the Injection Start Time to the Injection Stop Time.

(Optional) Moving and/or rotating injection release point parameters (available when Moving Injection

is enabled):

– The origin (X, Y, Z) and the direction of the axis (X, Y, or Z) about which the injection is rotating

– The Angular Velocity of the injection location

– The X, Y, Z components of the Translational Velocity of the injection location

At each time step, the MPM solver determines a new position of a particle injection based on

the injection origin at the previous time step and the specified translational velocities.

. Click Create/Modify.

The new injection that you have created appears under the Injections selection list.

.... Inputs for point Injections

For a point injection of a macroscopic particle, you need to define the following initial conditions in

the Create/Modify Injection dialog box:

Particle diameter

Particle density

Specific heat of the particle material (only for heat transfer simulations)

Initial particle temperature (only for heat transfer simulations)

Initial particle release location:

– Cartesian coordinates: X, Y, and Z

– Cylindrical coordinates: Radius, Angle, and Axial

Particle initial velocity:

– Cylindrical coordinates: Radial, Tangential, and Axial

Particle initial angular velocity

Cylindrical Coordinate System

By default, the global Cartesian coordinate system is used. If you want to specify injection parameters

in a local cylindrical coordinate system, enable the Cylindrical Coordinates option, and then define

the location of its origin (X, Y, Z) and Axis Direction.

.... Inputs for plane Injections

To define macroscopic particle injections released from a plane:

. Specify the particle initial conditions as described in Inputs for point Injections (p. ), except for the

particle release location. Note that for plane injections, velocities and initial position can be specified

only in Cartesian coordinates.

. Define the macroscopic particle injection plane.

Two options are available:

Rectangular

Macroscopic particles will be injected from a rectangular plane surface that is offset from a co-

ordinate plane by a distance specified in X, Y, or Z Position in the selected X, Y, or Z axis dir-

ection.

The minimum and maximum limits of the rectangular surface are defined under the Extents

of Rectangular Plane group box.

Circular

Macroscopic particles will be injected from a circular plane surface that is perpendicular to a

selected coordinate direction (X, Y, or Z). The origin and radius of the circle are specified under

the Center Location/Radius of Circular Plane group box.

. Define the distribution of the particle release locations.

Two modeling options are available:

Random

The MPM model will inject particles into a flow domain from random locations on the injection

plane. The total number of the released particles is specified in the Total # of Particles integer

entry field.

Uniform

The particles will be injected into a flow domain from points arranged in a rectangular pattern.

The number of the release points in two axial directions is specified in the appropriate integer

entry fields (for example, # of Particles in X-dir and # of Particles in Y-dir).

.... Inputs for packing Injections

To define an injection of macroscopic particles packed in a box or cylinder:

. Specify particle initial conditions as described in Inputs for point Injections (p. ), except for the

. Define the packing region.

For a Box-type packing, specify the minimum and maximum X, Y, and Z coordinates for the

packing bounding box under the Box Extents group box.

For a Cylinder-type packing, specify the bounding cylinder axis, minimum and maximum coordin-

ates for the cylinder height, cylinder origin and inner and out diameters.

. Define the particle distribution in the packing.

Random

The initial volume fraction of particles in the packing is specified in the Particle VOF entry field.

Uniform

The distance between particles in the initial spatially uniform packing is specified in the Inter

Particle Gap entry field.

. If you want to allow a part of the particle to be outside of the domain (with the particle center being in

the domain), enable Allow Partial Particles in the Domain.

.... Inputs for from-file Injections

For injections that you want to specify using the from-file option, the file format is:

number-of-particles

diameter density x-pos y-pos z-pos x-vel y-vel z-vel x-rot y-rot z-rot pstart pstop pinterval cemented

...

where the first line specifies the number of particles (number-of-particles), followed by number-

of-particles lines that define parameters for the injection particles. For each particle, you must

specify the diameter, density, initial position, linear and angular velocities, start, end, and interval

times, and the integer flag (cemented in the above file format specification) indicating whether or

not the particle is moving. Note that cemented= indicates a stationary particle, while cemented=

indicates a moving particle. Values describing an injection should be separated by one or more spaces

and can be specified using scientific notation (e or E) if needed.

All quantities are in SI units.

5e- .08e- -1e- 1e- .4e- -2e- 1e- . . . . . 1e- 1e-

The Attraction Forces tab allows you to include attraction forces between particles and walls in your

problem.

Figure . : Macroscopic Particle Model Dialog Box (Attraction Forces Tab)

To define the attraction forces between macroscopic particles:

. Select Enable Particle-Particle Forces.

. Specify the model constants n1, n2, n3, and G_p used in Equation ..

To define the attraction forces between macroscopic particles and walls:

. Select Enable Particle-Wall Forces.

. From the Participating Zones selection list, select the appropriate zones

. Specify the model constants n4, n5, and G_w used in Equation ..

The Initialize MPM tab allows you to apply macroscopic particle related source terms to the continuous

phase, initialize macroscopic particles, and display particle trajectories.

Figure . : Macroscopic Particle Model Dialog Box (Initialize MPM Tab)

You can also enable the following solution-related options:

Saving particle data in a Field View and/or ASCII format

Printing warning messages related to particle tracking in the Fluent console

Once you have set up the MPM model, you need to perform the following steps:

. Click Initialize MPM Functions.

This will set up macroscopic particle related source terms and apply them to the continuous phase.

It will also hook all appropriate UDF functions to the Fluent solver.

Initializing MPM functions adds the following two commands to the solver that will be executed

during simulation:

mpm1: displays the particle position(s) at each iteration step.

mpm3: writes the particle position(s) at each iteration step in PNG format.

You can disable these commands or modify the reporting frequency in the Execute Command

dialog box (accessible from the Solution/Calculation Activities/Execute Commands tree item).

If you want the solver to report or monitor additional solution quantities during calculation, you

can define your own execute command(s) using Fluent TUI commands. For more information, see

Executing Commands During the Calculation in the Fluent User's Guide (p. ).

For coupled simulations, once you click Initialize MPM Functions, the pressure discretization

scheme will automatically switch to PRESTO! to provide a more robust solution.

. Initialize either the macroscopic particles by clicking Initialize Particles or the flow field in the usual way

The macroscopic particle(s) will be introduced into the fluid flow during the next computational

time step.

. Run the simulation with the injected macroscopic particle(s).

Upon completion of the MPM simulation, you can click Display Injections... and use the Display

Particles dialog box to display the computed particle trajectories.

In the Display Particles dialog box, you can select the particle coloring option. You can color particle

by the following particle variable values:

diameter

mass

particle ID

velocity magnitude

For the Particle Velocity Magnitude option, you can specify the minimum and maximum range of

the velocity magnitude values.

Chapter : Modeling Multiphase Flows

This chapter discusses the general multiphase models that are available in ANSYS Fluent. For information

about the various theories behind the general multiphase models in ANSYS Fluent, see Multiphase

Flows in the Theory Guide. Information about using the general multiphase models in ANSYS Fluent is

The first step in solving any multiphase problem is to determine which of the regimes described in

Multiphase Flow Regimes in the Theory Guide best represents your flow.Model Comparisons in the

Theory Guide provides some broad guidelines for determining appropriate models for each regime,

and Detailed Guidelines provides details about how to determine the degree of interphase coupling

for flows involving bubbles, droplets, or particles, and the appropriate model for different amounts of

coupling.

The following sections will guide you through the setup, solution, and postprocessing of multiphase

flow models.

.. Steps for Using a Multiphase Model

coupling.

The procedure for setting up and solving a general multiphase problem is outlined below, and described

in detail in the subsections that follow. Remember that only the steps that are pertinent to general

multiphase calculations are shown here. For information about inputs related to other models that you

are using in conjunction with the multiphase model, see the appropriate sections for those models.

See also Additional Guidelines for Eulerian Multiphase Simulations (p. ) for guidelines on simplifying

Eulerian multiphase simulations.

Important

Double Precision is recommended for all multiphase cases.

. Enable the multiphase model you want to use (VOF, mixture, or Eulerian) and specify the number of phases.

For the VOF and Eulerian models, specify the volume fraction scheme as well.

Setup →

Models →

Multiphase → Edit...

See Enabling the Multiphase Model (p. ) and Choosing Volume Fraction Formulation (p. ) for

details.

. Copy the material representing each phase from the materials database.

Setup →

Materials

If the material you want to use is not in the database, create a new material. See Using the Cre-

ate/Edit Materials Dialog Box (p. ) for details about copying from the database and creating new

materials. See Modeling Compressible Flows (p. ) for additional information about specifying

material properties for a compressible phase. It is possible to turn off reactions in some materials

by selecting none in the Reactions drop-down list under Properties in the Create/Edit Materials

Important

Important

If your model includes a particulate (granular) phase, you will need to create a new ma-

terial for it in the fluid materials category (not the solid materials category).

. Define the phases, and specify any interaction between them (for example, surface tension if you are using

the VOF model, slip velocity functions if you are using the mixture model, or drag functions if you are using

the Eulerian model).

Setup → Models → Multiphase → Phases

Edit...

See Defining the Phases (p. ) – Defining the Phases for the Eulerian Model (p. ) for details.

. (Eulerian model only) If the flow is turbulent, define the multiphase turbulence model.

Setup →

Models →

See Modeling Turbulence (p. ) for details.

. If body forces are present, enable gravity and specify the gravitational acceleration.

Setup →

See Including Body Forces (p. ) for details.

. Specify the boundary conditions, including the secondary-phase volume fractions at flow boundaries and

(if you are modeling wall adhesion in a VOF simulation) the contact angles at walls.

Setup →

See Defining Multiphase Cell Zone and Boundary Conditions (p. ) for details.

. Set any model-specific solution parameters.

Solution →

Methods

Solution →

Controls

See Setting Time-Dependent Parameters for the Explicit Volume Fraction Formulation (p. ) and

Solution Strategies for Multiphase Modeling (p. ) for details.

. Initialize the solution and set the initial volume fractions for the secondary phases.

Modeling Multiphase Flows

Patch...

Patch...

See Setting Initial Volume Fractions (p. ) for details.

. Calculate a solution and examine the results. Postprocessing and reporting of results are available for each

phase that is selected.

See Solution Strategies for Multiphase Modeling (p. ) and Postprocessing for Multiphase Model-

Note

For information on multiphase model compatibility with other Fluent models, see Appendix A: AN-

SYS Fluent Model Compatibility (p. ).

If the multiphase model is used in combination with a species model, the mass fraction of a

species may be displayed incorrectly in ANSYS CFD-Post if the volume fraction of a cell is zero.

This applies for all ANSYS Fluent files written prior to release  R3.

species as an additional quantity to be saved in the data file (through the Data File

Quantities dialog box).

This section provides instructions and guidelines for using the VOF, mixture, and Eulerian multiphase

models.

Information is presented in the following subsections:

... Enabling the Multiphase Model

... Choosing Volume Fraction Formulation

... Solving a Homogeneous Multiphase Flow

...The Boussinesq Approximation in Multiphase Flow

... Modeling Compressible Flows

... Defining the Phases

... Including Body Forces

... Modeling Multiphase Species Transport

... Specifying Heterogeneous Reactions

... Including Mass Transfer Effects

... Defining Multiphase Cell Zone and Boundary Conditions

... Setting Initial Volume Fractions

To enable the VOF, mixture, or Eulerian multiphase model, select Volume of Fluid, Mixture, or Eulerian

under Model in the Multiphase Model Dialog Box (p. ).

Setup →

Models →

The dialog box will expand to show the relevant inputs for the selected multiphase model.

Steps for Using a Multiphase Model

Volume of Fluid Model Inputs

Figure . : Multiphase Model Dialog Box for the VOF Model

Number of Eulerian Phases

(optional) Coupled Level Set + VOF (see Coupled Level-Set and VOF Model in the Theory Guide)

volume fraction Formulation (Explicit or Implicit) and associated parameters (see Choosing Volume

Fraction Formulation (p. ))

(optional) inclusion of sub-models such as Open Channel Flow and Open Channel Wave BC

Interface Modeling type and options (see Choosing Volume Fraction Formulation (p. ))

(optional) selection of Expert Options (see Expert Options (p. ))

(optional) inclusion of the Implicit Body Force formulation (see Including Body Forces (p. ))

Mixture Model Inputs

Figure . : Multiphase Model Dialog Box for the Mixture Model

(optional) inclusion of Slip Velocity (see Solving a Homogeneous Multiphase Flow (p. ))

Eulerian Model Inputs

Figure . : Multiphase Model Dialog Box for the Eulerian Model

(optional) inclusion of the Dense Discrete Phase Model

(optional) inclusion of the Boiling Model

(optional) inclusion of the Multi-Fluid VOF Model

Interface Modeling type and options (see Choosing Volume Fraction Formulation (p. )).This is only

available if the Multi-Fluid VOF Model is enabled.

To specify the number of phases for the multiphase calculation, enter the appropriate value in the

Number of Eulerian Phases field. You can specify up to  phases.

ANSYS Fluent supports the following options for volume fraction formulation:

Explicit Formulation

The explicit formulation is non-iterative and is time-dependent.Thus it can only be used with the

Transient solver. It exhibits better numerical accuracy compared to the implicit formulation. However

the time step size is limited by a Courant-based stability criterion.

Implicit Formulation

The implicit formulation is iterative and can be used with either the Steady or Transient solver. It

is well-suited to steady-state applications as the solution information propagates much faster com-

pared to the explicit formulation.

For steady-state flow applications, either a steady-state or a transient simulation may be required, de-

pending on the characteristics of the flow:

Steady-state simulation: If the final steady-state solution is not affected by the initial flow conditions

and there is a distinct inflow boundary for each phase.

Transient simulation: If the final steady-state solution is dependent on the initial flow conditions and/or

you do not have a distinct inflow boundary for each phase.

For transient flow applications, the implicit formulation may allow you to use a much larger time step

than the explicit formulation due to the implicit formulation’s unconditional stability. However, the

implicit time-step size may be limited by truncation errors. The implicit formulation produces more

numerical diffusion than the explicit formulation when using the First Order transient formulation.

Therefore, the implicit formulation should be used along with higher-order transient formulations to

achieve better numerical accuracy.

To specify the volume fraction formulation to be used for the VOF and Eulerian multiphase models,

select the appropriate Formulation under Volume Fraction Parameters in the Multiphase Model

.... Interface Modeling Type

For the VOF and Mixture multiphase models and for the Eulerian multiphase model with Multi-Fluid

VOF enabled, you must specify the interface regime that you will be modeling. This will determine

the availability of the various volume fraction discretization schemes (Spatial Discretization Schemes

for Volume Fraction (p. )). The following options are available for Interface Modeling Type:

Sharp

(VOF and Multi-Fluid VOF models only) for when a distinct interface is present between the phases

Dispersed

for when the phases are interpenetrating

Sharp/Dispersed

a hybrid approach for flows consisting of both sharp and dispersed interfaces.This option can also

be used to capture mildly sharp interfaces. Mildly sharp interfaces are those that are neither as sharp

as would be captured by the schemes available with the Sharp option, nor as diffused as would be

captured by the schemes available with the Dispersed option.

Interfacial Anti-Diffusion

If you are using the Sharp interface modeling type, you can optionally enable the Interfacial Anti-

Diffusion treatment. This treatment is applied only in interfacial cells and attempts to suppress the

numerical diffusion that can arise from the volume fraction advection schemes.

The use of this treatment can have adverse effects on convergence, especially with aggressive settings

and large time step size. Therefore, it should be used in cases that use a coarse mesh, that have high

aspect-ratio cells, that have large cell-volume jumps in the vicinity of the fluid-fluid interface, or that

suffer from excess numerical diffusion.

The strength of the anti-diffusion treatment can be specified using the define/models/mul-

tiphase/interface-modeling-options text command. The strength can range between

(none) and  (maximum).

Sharp/Dispersed Interface Modeling Options

Selecting Sharp/Dispersed will make available some additional discretization options. To access these,

click Interface Modeling Options... in the Multiphase Model dialog box.

These options allow you to adjust the discretization behavior on a per-zone and/or per-phase-pair

basis for cases in which it is important to simultaneously model dispersed and sharp interfaces.

Zonal Discretization

This option is appropriate for applications that require either sharp or dispersed interface modeling

depending on the cell zone. After enabling Zonal Discretization you will need to specify the slope

limiter value on the Multiphase tab of the Fluid dialog box for each cell zone. (See Defining Multiphase

Cell Zone and Boundary Conditions (p. ))

Phase Localized Discretization

depending on the phase-pair comprising the interface. After enabling Phase Localized Discretization

you will need to specify the slope limiter values for each phase pair on the Discretization tab of the

Phase Interaction dialog box.

.... Spatial Discretization Schemes for Volume Fraction

You can choose from various spatial discretization schemes for volume fraction depending on the

multiphase model in use, the interface regime type, and the volume fraction formulation chosen. The

available discretization schemes for each combination of model, formulation, and interface regime

are summarized in the following tables:

Table . : Spatial Discretization Schemes for the VOF and Eulerian with Multi-Fluid VOF Models

Interface Modeling Type

Geo-Reconstruct

CICSAM

CICSAM

Compressive

BGM (steady state only)

Modified HRIC

Sharp

First Order Upwind

QUICK

Second Order Upwind

QUICK

Dispersed

Table . : Spatial Discretization Schemes for the Eulerian Model without Multi-Fluid VOF

QUICK

QUICK

Table . : Spatial Discretization Schemes for the Mixture Model

QUICK

Dispersed

The Geo-Reconstruct scheme is an interface tracking scheme based on geometrical information. It

is the most accurate scheme, but is more computationally expensive than the other schemes. Geo-

Reconstruct is the preferred scheme when solving on meshes of poor quality.

The CICSAM, Modified HRIC, and Compressive schemes are interface capturing schemes based on

algebraic information.

The Donor-Acceptor discretization is a scheme applicable only to quad- and hex-meshes. As it is

considered obsolete, it does not appear by default in the graphical user interface. However, it can be

made available if required using the following text command:

/solve/set/expert

<...>

Allow selection of all applicable discretization schemes? [no] yes

This command can also be used to expose discretization schemes that may be applicable, but are

hidden by default according to the tables above.

Important

Important

For the geometric reconstruction and donor-acceptor schemes, if you are using a conformal

mesh (that is, if the mesh node locations are identical at the boundaries where two subdo-

mains meet), you must ensure that there are no two-sided (zero-thickness) walls within

the domain. If there are, you will need to slit them, as described in Slitting Face

For more details about the implementations of the volume fraction discretization schemes, refer to

Interpolation Near the Interface in the Fluent Theory Guide.

....Volume Fraction Limits

The Volume Fraction Cutoff allows you to specify a cutoff limit for the volume fraction values. The

value that you provide is used as the lower cutoff for the volume fraction. All volume fraction values

in the domain below this cutoff value are set to zero. The upper cutoff is calculated as (. - lower

cutoff). All volume fraction values above the upper cutoff value are set to .. The default value is

1e-, which is the recommended value. Using a higher value may lead to a higher volume imbalance.

Important

The Volume Fraction Cutoff value can be specified only with the Explicit formulation

for volume fraction.

Note

For the Implicit formulation, the minimum value allowed is  and the maximum al-

lowable value is 1e-. For the Explicit formulation, the minimum value allowed is

and the maximum allowable value is 1e-. A higher cutoff value is available with the

Explicit formulation because it allows for the local redistribution procedure of partially

filled cells, which accounts for volume loss. This treatment is not available with the

Implicit formulation.

.... Expert Options

When using the Explicit formulation, there are several additional options that you can access by

clicking Expert Options... in the Multiphase Model dialog box.

Sub-Time Step Calculation Method

This setting controls how the time-scale is computed when determining the time step used for volume

fraction.

Solve VOF Every Iteration

This setting controls whether to solve the volume fraction equations once per iteration, or only once

per time step.

For a more detailed discussion of how to use these options, refer to Setting Time-Dependent Para-

meters for the Explicit Volume Fraction Formulation (p. ).

If you are using the mixture model, you have the option to disable the calculation of slip velocities

and solve a homogeneous multiphase flow (that is, one in which the phases all move at the same ve-

locity). By default, ANSYS Fluent will compute the slip velocities for the secondary phases, as described

in Relative (Slip) Velocity and the Drift Velocity in the Theory Guide. If you want to solve a homogeneous

multiphase flow, turn off Slip Velocity under Mixture Parameters.

When using the Boussinesq approximation for density variation in multiphase flows, there are several

important items to consider:

The Boussinesq approximation is only valid for small variations in fluid densities caused by small variations

in temperature.Therefore, constant density is assumed, and a momentum source is only added for modeling

buoyancy.

buoyancy.

The Boussinesq approximation assumes that small density variations have little effect on inertial terms and

strong effects on gravitational terms.Thus, the differences in specific weights between two fluids or layers

of fluids is the force driving the flow. (Waves cannot use this approximation.) Two non-dimensional numbers

quantify the effect of buoyancy: the Richardson number and the Rayleigh number.

Operating density should be set to zero.

For additional information on the Boussinesq approximation, see The Boussinesq Model (p. ).

If you are using any of the multiphase models for a compressible flow, note the following:

ANSYS Fluent allows the modeling of:

– Multiple compressible ideal gas phases and/or incompressible/compressible liquids at any inlet

– A single real gas or real liquid at any inlet

– Multiple real gases at a single inlet

– Multiple compressible liquids using either the Fluent built-in compressible liquid density model based

on the Tait law (see Compressible Liquid Density Method (p. )) or user-defined functions

For multiple compressible phases, the fundamental equations for compressible flow remain the

same. However, boundary conditions are modified to account for changes in material properties

due to compressible fluid mixtures.

In cases of a mixture of ideal and real gases, the phases must enter the domain through separate inlets.

When using the VOF model, stability is improved if the primary phase is the compressible ideal gas.

If you specify the total pressure at a boundary (for example, for a pressure inlet or intake fan), Fluent  will

use the specified value for temperature at that boundary as total temperature for the compressible phase,

and as static temperature for the other phases (which are incompressible).

For each mass-flow inlet, you will need to specify mass flow or mass flux for each individual phase.

Important

Note that if you read a case file that was set up in a version of Fluent  previous to .,

you will need to redefine the conditions at the mass-flow inlets. See Defining Multiphase

Cell Zone and Boundary Conditions (p. ) for more information on defining conditions

for a mass-flow inlet in multiphase calculations.

Enhanced Compressible Flow Numerics

Compressible flow simulations may have convergence difficulties due to explicit handling of source

term accounting for density variation. These simulations could become extremely unstable in the

presence of a large variation in pressure and temperature. In ANSYS Fluent, an enhanced numerical

treatment that provides better stability at startup and during calculation of compressible flows is enabled

by default. The treatment controls the rate of change of pressure and temperature between iterations

and provides additional diagonal dominance to the matrix of equations.

Although disabling the enhanced numerical treatment is not recommended, you can temporarily turn

it off to investigate unstable cases using the following text user interface command:

solve/set/multiphase-numerics/compressible-flow/enhanced-numerics

...

enhanced compressible flow numerics? [yes] no

See Compressible Flows (p. ) for more information about compressible flows.

Alternative Compressible Flow Numerics

...

A more general formulation for compressible multiphase flows employs a mathematically rigorous

treatment of compressible phases at an inlet boundary. Instead of treating the entering incompressible

and compressible phases as a pseudo-mixture, this formulation calculates static temperature and

pressure using an iterative method based on fundamental thermodynamic relations (such as the

Maxwell relations). This approach involves evaluation of the property derivatives, which can be computed

either numerically or through analytic expressions. You can enable this alternative treatment via the

solve/set/multiphase-numerics/compressible-flow/alternate-bc-formulation

alternate compressible bc formulation? [no] y

use analytical thermodynamic derivatives? [no] y

To define the phases (including their material properties) and any interphase interaction (for example,

surface tension and wall adhesion for the VOF model, slip velocity for the mixture model, drag functions

for the mixture and the Eulerian models), (Figure . : The Phases Dialog Box (p. )).

Edit...

Figure . : The Phases Dialog Box

Each item in the Phases list in this dialog box is one of two types: a Primary-Phase indicates that the

selected item is the primary phase, and Secondary-Phase indicates that the selected item is a secondary

phase. To specify any interaction between the phases, click the Interaction... button.

Instructions for defining the phases and interaction are provided in Defining the Phases for the VOF

Model (p. ), Defining the Phases for the Mixture Model (p. ), and Defining the Phases for the Eu-

lerian Model (p. ) for the VOF, mixture, and Eulerian models, respectively.

When large body forces (for example, gravity or surface tension forces) exist in multiphase flows, the

body force and pressure gradient terms in the momentum equation are almost in equilibrium while

the contributions of convective and viscous terms are small in comparison. Segregated algorithms

converge poorly unless partial equilibrium of pressure gradient and body forces is taken into account.

ANSYS Fluent provides an optional “implicit body force” treatment that can account for this effect,

making the solution more robust.

The basic procedure involves augmenting the correction equation for the face flow rate, Equation .

in the Theory Guide, with an additional term involving corrections to the body force. This results in

extra body force correction terms in Equation . in the Theory Guide, and allows the flow to achieve

a realistic pressure field very early in the iterative process.

To include this body force, enable Gravity in the Operating Conditions Dialog Box (p. ) and specify

the Gravitational Acceleration.

Setup →

For VOF calculations, you should also enable the Specified Operating Density option in the Operating

Conditions dialog box, and set the Operating Density to be the density of the lightest phase. (This

excludes the buildup of hydrostatic pressure within the lightest phase, improving the round-off accuracy

for the momentum balance.) If any of the phases is compressible, set the Operating Density to zero.

Important

For VOF and mixture calculations involving body forces, it is recommended that you also

enable the Implicit Body Force treatment for the Body Force Formulation in the Mul-

tiphase Model dialog box. This treatment improves solution convergence by accounting

for the partial equilibrium of the pressure gradient and body forces in the momentum

equations. See Including Body Forces (p. ) for details.

ANSYS Fluent lets you describe a multiphase species transport and volumetric reaction (Modeling

Species Transport in Multiphase Flows in the Theory Guide) in a fashion that is similar to setting up a

single-phase chemical reaction using the Species Model dialog box (for example, Figure . : The

Species Model Dialog Box with a Multiphase Model Enabled (p. )).

Setup →

Models →

Species → Edit...

Figure . : The Species Model Dialog Box with a Multiphase Model Enabled

. Select Species Transport under Model.

. Select a specific phase using the Phase drop-down list under Phase Properties.

. Click the Set... button to display the Phase Properties dialog box (Figure . :The Phase Properties

Figure . : The Phase Properties Dialog Box

In the Phase Properties dialog box, the material for each phase is listed in the Material drop-down

list. From this list, you can choose the material that you want to use for a specific phase. The drop-

down list contains all of the materials, then open the Edit Material dialog box by clicking the

Edit... (or View...) button next to the Material drop-down list.

. In the Species Model dialog box, choose the Turbulence-Chemistry Interaction model.Three models

chemistry interaction.

Eddy-Dissipation

(for turbulent flows) computes only the mixing rate (see Equation . and Equation . in the Theory

Guide).

Finite-Rate/Eddy-Dissipation

(for turbulent flows) computes both the Arrhenius rate and the mixing rate and uses the smaller of

the two.

When modeling multiphase species transport, additional inputs may also be required depending on

your modeling needs. See, for example, Specifying Heterogeneous Reactions (p. ) for more inform-

ation defining heterogeneous reactions, or Including Mass Transfer Effects (p. ) for more information

on mass transfer effects.

You can use ANSYS Fluent to define multiple heterogeneous reactions and stoichiometry using the

Phase Interaction dialog box (for example, Figure . : The Phase Interaction Dialog Box for Hetero-

geneous Reactions (p. )).

Edit... → Interaction...

. In the Phases dialog box (Figure . :The Phases Dialog Box (p. )), click the Interaction... button to

open the Phase Interaction dialog box.

Figure . : The Phase Interaction Dialog Box for Heterogeneous Reactions

. Click the Reactions tab in the Phase Interaction dialog box.

. Set the total number of reactions (volumetric reactions, wall surface reactions, and particle surface reactions)

in the Total Number of Heterogeneous Reactions field. (Use the arrows to change the value, or type in

the value and press Enter.)

. Enable the Heterogeneous Stiff Chemistry Solver option if your inter-phase reaction mechanism contains

numerically stiff reactions.This option can improve convergence and is available for transient Eulerian

multiphase simulations.When this option is enabled, ANSYS Fluent uses a fractional step algorithm where

the flow is advanced without reaction sources for a time step, and then the chemistry is integrated point-

by-point for the same time step.The stiff chemistry scheme solves all species in all phases coupled. Note

that it is possible to include homogeneous (intra-phase) reactions along with the heterogeneous reactions

in the (Phase Interaction dialog box (instead of in the reaction mechanism in the Create/Edit Materials

dialog box), and these reactions will be solved with the stiff solver.The stiff ODE solver tolerances can be

set using the following text command:

solve → set → heterogeneous-stiff-chemistry

. Specify the Reaction Name of each reaction that you want to define.

. Set the ID of each reaction you want to define. (Again, if you type in the value be sure to press Enter.)

. For each reaction, specify how many reactants and products are involved in the reaction by increasing

the value of the Number of Reactants and the Number of Products. Select each reactant or product in

the Reaction tab and then set its stoichiometric coefficient in the Stoich. Coefficient field. (The stoi-

chiometric coefficient is the constant

or

in Equation . in the Theory Guide.)

. For each reaction, indicate the Phase and Species and the stoichiometric coefficient for each of your re-

actants and products.

. For each reaction, use the Reaction Rate Function drop-down list to select one of the following:

none

if you do not want to include a reaction rate

population-balance

is the mass transfer due to nucleation and growth. If neither the primary phase or secondary phase

has species associated with it, then the mass transfer is modeled as unidirectional. If the mass transfer

process involves reactions or species, the problem must be set up as one involving heterogeneous

reaction/mass transfer.

Important

The population-balance option for Reaction Rate Function should not be used if

there are multiple reactions leading to the formation of the secondary phase. In this

case, the reaction rate functions should be specified either through the standard

dialog boxes or user-defined functions and the growth rate function should be a

sum of the individual reaction rates. This would ensure consistency between the

individual reaction rates and the total mass transfer from the primary to the secondary

phase.

You can always use DEFINE_MASS_TRANSFER or DEFINE_HET_RXN_RATE user-defined

phase.

function types instead of the population-balance option to specify mass transfer rates. However,

the growth rate function and the mass transfer rates returned from the UDFs need to be con-

sistent with each other.

arrhenius-rate

to specify rate exponents for an Arrhenius-type reaction (see Heterogeneous Phase Interaction in the

Theory Guide for more information)

Important

This simple form of the Arrhenius rate option may only be used for devolatilization

reactions only. Char combustion reaction may be more involved and complicated

to be simply casted in this form. Additional diffusion rate formulations may be needed

to formulate a complete char (or solid phase) reaction system.

Important

Note that you can also specify the heterogeneous reaction rates using a user-defined

function. A user-defined function is available for an Arrhenius-type reaction with rate

exponents that are equivalent to the stoichiometric coefficients. For more information,

see DEFINE_HET_RXN_RATE in the Fluent Customization Manual.

Important

ANSYS Fluent assumes that the reactants are mixed thoroughly before reacting together,

therefore the heat and momentum transfer is based on this assumption. This assumption

can be disabled using a text command. For more information, contact your ANSYS Fluent sup-

port engineer.

As discussed in Modeling Mass Transfer in Multiphase Flows in the Theory Guide, mass transfer effects

in the framework of ANSYS Fluent’s general multiphase models (that is, Eulerian multiphase, mixture

multiphase, or VOF multiphase) can be modeled in one of three ways:

Unidirectional constant rate mass transfer

UDF-prescribed mass transfer

mass transfer through cavitation, evaporation-condensation, boiling, or generalized species mass transfer

Because of the different procedures and limitations involved, defining mass transfer through the

Singhal et al. cavitation model is described separately in Including Cavitation Effects (p. ).

Note

There are limitations and recommendations specific to using cavitation with the VOF model.

See Limitations of Cavitation with the VOF Model in the Fluent Theory Guide for additional

For general limitations regarding the cavitation models, see Limitations of the Cavitation

To define mass transfer in a multiphase simulation as a unidirectional constant, using a user-defined

function, through population balance, cavitation, evaporation/condensation, or species mass transfer

you will need to use the Phase Interaction dialog box (for example, Figure . : The Phase Interaction

Dialog Box for Mass Transfer (p. )).

Figure . : The Phase Interaction Dialog Box for Mass Transfer

. Click the Mass tab in the Phase Interaction dialog box.

. Specify the Number of Mass Transfer Mechanisms.

Important

In general, you should use only one mass transfer mechanism when you employ one of

the available mass transfer models (see Step ). Although using multiple mass transfer

mechanisms is allowed for any pairs of phases (including the same pair of phases), it is

not recommended because the mass transfer models have been fundamentally developed

for a single mass transfer process. These models do not account for possible interactions

between two mass transfer mechanisms in a flow system. In order to account for all

relevant physics using UDFs in multiple mass transfer mechanisms, you can use the user-

defined option. For additional restrictions when using multiple mass transfer mechanisms,

see Step .

. For each mechanism, specify the phase of the source material under From Phase. Note that the phase

you select for From Phase must be a liquid if you plan to select cavitation, evaporation-condensation,

or boiling from the Mechanism drop-down menu (see Step ).

. If species transport is part of the simulation, and the source phase is composed of a mixture material, then

specify the species of the source phase mixture material in the corresponding Species drop-down list.

. For each mechanism, specify the phase of the destination material phase under To Phase. Note that the

phase you select for To Phase must be a vapor if you plan to select cavitation, evaporation-condensation,

or boiling from the Mechanism drop-down menu. If you plan to select species-mass-transfer and one

of the phases is a gas, it must be specified as the To Phase (see Step ).

. If species transport is part of the simulation, and the destination phase is composed of a mixture material,

then specify the species of the destination phase mixture material in the corresponding Species drop-

down list.

down list.

. For each pair of phases with mass transfer, select the desired mass transfer mechanism under Mechanism.

The available mechanisms and their inputs are described in Mass Transfer Mechanisms (p. ).

ANSYS Fluent will automatically include the terms needed to model mass transfer in all relevant

conservation equations. Another option to model mass transfer between phases is through the

use of user-defined sources and their inclusion in the relevant conservation equations. This approach

is more involved, but more powerful, allowing you to split the source terms according to a model

of your choice.

Important

Except for the species-mass-transfer mechanism, if the same mass transfer model is selected

for multiple mass transfer mechanisms, the most recently edited mechanism sub-model, including

its parameters, options, and constants (excluding its material properties, such as vaporization

pressure or saturation temperature), will apply to all the mass transfer mechanisms.

When modeling multiple species-mass-transfer mechanisms, you can select different species

mass transfer models and model options, such as Raoult's Law, Henry's Law, etc. However, because

there is a lack of interaction between different species mass transfer models, this should be

done with caution. For information on modeling restrictions for interphase species mass transfer,

see Interphase Species Mass Transfer in the Fluent Theory Guide.

Momentum, energy, and turbulence are also transported with the mass that is transferred. ANSYS

Fluent assumes that the reactants are mixed thoroughly before reacting together, therefore the

heat and momentum transfer is based on this assumption.This assumption can be disabled

using a text command. For more information, contact your ANSYS Fluent support engineer.

When your model involves the transport of multiphase species, you can define a mass transfer mech-

anism between species from different phases. If a particular phase does not have a species associated

with it, then the mass transfer throughout the system will be performed by the bulk fluid material.

Important

Including species transport effects in the mass transport of multiphase simulation requires

that Species Transport be selected in the Species Model dialog box.

Setup →

Models →

Species

.... Alternative Modeling of Energy Sources

The existing formulation of sensible enthalpy for interphase mass transfer includes the formation

enthalpy, which could be problematic for some cases, such as cases that involve species transport

and reactions. The alternative treatment, which is available with the VOF and Mixture multiphase

models, is based on the explicit modeling of the energy source driven by mass transfer. You can enable

the alternative formulation by using the following text command:

solve/set/multiphase-numerics/heat-mass-transfer/alternative-energy-

treatment?

enable alternative treatment of handling latent heat source [no] y

Energy Source Treatment

The energy source is modeled explicitly as:

(.)

where

is the mass transfer rate, and  is latent heat of vaporization. If you are using the tabular-

(.)

where

ptl-sat method to specify saturation temperature for the Evaporation-Condensation Mechanism (p. )

or vaporization pressure for the Cavitation Mechanism (p. ), ANSYS Fluent will take the latent heat

values directly from the tabular data. Otherwise, it is calculated as:

(.)

Here,

and

are saturation enthalpies of phase  and phase  at the saturation temperature, re-

spectively. They are calculated as:

(.)

(.)

where,

and

= formation enthalpies of phase  and phase , respectively

and

= specific heats of phase  and phase , respectively

and

= reference temperatures of phase  and phase  as specified in the

Create/Edit Materials dialog box, respectively.

= saturation temperature

Note

For mass transfer mechanisms that do not require explicit input of saturation temperature,

such as cavitation and species mass transfer, the saturation temperature is assumed as the

reference temperature of the liquid.

Sensible Enthalpy Definition

For mass transfer cases, ANSYS Fluent by default uses the following definition of sensible enthalpy:

(.)

where,

= sensible enthalpy of phase

= formation enthalpy of phase

= specific heat of phase

= temperature of phase

= reference temperature of phase  as specified in the Create/Edit Materials

dialog box

The alternative treatment considers the definition of sensible enthalpy that excludes formation enthalpy.

Sensible enthalpy for each phase is expressed as:

(.)

with

=. K.

Heat Flux Reporting Strategies

When you use the alternative formulation, the following additional variable become available for

(.)

with

=. K.

postprocessing under the Phase Interaction... category:

In the variable selection drop-down lists that appear in postprocessing dialog boxes, this quantity

will be appended with the ID of the corresponding mass transfer mechanism.

Due to the explicit nature of the alternative formulation, the latent heat source appears as the heat

imbalance in heat flux reporting.

If you want to know the heat imbalance due to the latent heat source, you should create a custom-

field function for the mass transfer rate multiplied by latent heat, and then report it as a volume in-

tegral. ANSYS Fluent will report the following value:

(.)

where,

= heat imbalance

= number of mass transfer mechanisms that you defined

= mass transfer rate of

th mechanism

= Latent heat of

= volume

.... Mass Transfer Mechanisms

When including mass transfer effects in a multiphase simulation, you can choose from the following

mechanisms for each phase pair that undergoes mass transfer:

constant-rate

cavitation

evaporation-condensation

species-mass-transfer

boiling

Details for each mechanism are provided in the following sections:

..... Constant-Rate Option

..... User-Defined Option

..... Population-Balance Mechanism

..... Cavitation Mechanism

..... Evaporation-Condensation Mechanism

..... Species-Mass-Transfer Mechanism

..... Boiling Mechanism

You can use the constant-rate option to specify a constant value for unidirectional mass transfer.

The constant-rate must be entered in units of /time unit.

The user-defined option allows you to implement a correlation reflecting a model of your choice,

through a user-defined function.

With the population-balance mechanism, you can model flow where a number density function is

introduced to account for the particle population. With the aid of particle properties (for example,

particle size, porosity, composition, and so on), different particles in the population can be distin-

guished and their behavior can be described. For a comprehensive understanding of this option,

refer to the Population Balance Module Manual.

The cavitation mechanism allows you to select a cavitation model. For a cavitating flow, it is recom-

mended that you select liquid as the primary phase and vapor as the secondary phase.

The cavitation models are available when using mixture, VOF, and Eulerian multiphase models. You

are provided with two model options: Schnerr-Sauer and Zwart-Gerber-Belamri. To open the

Cavitation Model dialog box, select cavitation from the Mechanism drop-down list. For information

about the cavitation models, refer to Cavitation Models in the Theory Guide.

Figure . : The Cavitation Model Dialog Box

For the Schnerr-Sauer model, specify the Bubble Number Density (

Theory Guide) under Model Constants.The default value of 1e11 is suitable for most cases.

For the Zwart-Gerber-Belamri model, specify the Bubble Diameter, the Nucleation Site Volume

Fraction, the Evaporation Coefficient, and the Condensation Coefficient under Model Constants.

Under Cavitation Properties, specify the Vaporization Pressure and, if desired, a temperature depend-

ence function. In addition to the methods described in Defining Properties Using Temperature-Dependent

Functions (p. ) (constant, polynomial, piecewise-linear, piecewise-polynomial, or user-defined),

you can choose one of the following:

– taylor-approximation

The taylor-approximation method models the vaporization pressure as linearly varying with

temperature about the free-stream value. This approach can improve numerical stability, but is

only appropriate when deviations about the free-stream temperature are sufficiently small that

higher-order terms can be neglected. The expression for the vaporization pressure using the

taylor-approximation method is:

(.)

where

is the free-stream temperature,

is the latent heat, and

is a user-modifiable

coefficient. In the Taylor Approximation dialog box, you will specify Vaporization Pressure

(at the free-stream temperature), Free Stream Temperature, and Thermal Coefficient (

).

– tabular-pt-sat

This method allows you to specify vaporization pressure using a table that contains data points

for saturation temperature and saturation pressure. Saturation pressure will be interpolated

based on the static temperature from the solution, which is assumed to be at a saturated state.

The table format is described in Specifying Variables in a Tabular Format (p. ). Once you select

tabular-pt-sat, the Table Input dialog box opens where you can select the appropriate table

and the names of the columns from the Saturation Temperature and Saturation Pressure

selection lists.

Figure . : Table Input for Vaporization Pressure

– tabular-ptl-sat

(available only with Alternative Modeling of Energy Sources (p. )) The method allows you to

specify saturation pressure using a table that contains data points for saturation temperature,

saturation pressure, and latent heat. Saturation pressure and latent heat will be interpolated

tabular-ptl-sat, the Table Input dialog box opens where you can select the appropriate table

and the names of the columns from the Saturation Temperature, Saturation Pressure and

Latent Heat selection lists.

Note

If you are using tabular-pt-sat or tabular-ptl-sat to specify vaporization pressure, you

must first read an appropriate table following the procedure outlined in Specifying

Variables in a Tabular Format (p. ). All table data must be in SI units (saturation

temperature in Kelvin (K), saturation pressure in Pascal (Pa), and latent heat in Joule/Kg).

If you want to include the influence of turbulence on the threshold cavitation pressure, enable Turbulence

Factor. If desired, you can adjust the value of the Turbulent Coefficient. For details about the imple-

mentation of the Turbulence Factor, see Turbulence Factor in the Fluent Theory Guide.

By default, the minimum vapor pressure limit is set to  Pa. The default value for the maximum vapor

pressure limit is set to five times the local vapor pressure with consideration of the turbulent and

thermal effects for each computational cell and phase. The default and recommended value for the

evaporation and condensation coefficients in the Schnerr-Sauer model (

and

in Equa-

tion . in the Fluent Theory Guide) are  and ., respectively. You can modify these default values

using the following expert text commands:

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/min-vapor-

pressure

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/max-vapor-

pressure-ratio

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/schnerr-cond-

coeff

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/schnerr-evap-

coeff

Note

If you use multiple cavitation mass transfer mechanisms in your simulation, the value you

specify for Turbulence Factor will automatically apply to all cavitation mechanisms, thereby

overwriting previously existing turbulent coefficients.

If the Mixture multiphase model is enabled, then the Singhal et al. cavitation model can be

enabled using the solve/set/expert text command and responding yes to use

Singhal-et-al cavitation model?.The Singhal-Et-Al Cavitation Model option

will now be visible in the Phase Interaction dialog box, under the Mass tab. Enable this option

to include the Singhal et al. cavitation model. Refer to Including Cavitation Effects (p. ) for

information about setting the cavitation parameters. Also refer to Cavitation Models in the

Theory Guide for information about the Singhal et al. model.

To disable this model, first deselect the Singhal-Et-Al Cavitation Model option in the

Phase Interaction dialog box, then type the solve/set/expert text command

again and enter no when asked if you want to use Singhal-et-al cavitation

model?

For turbulent flows, if one of the phases participating in cavitation is primary, then ANSYS Fluent

automatically enables the generalized turbulent diffusion treatment. The treatment adds a diffusion

source in the volume fraction equation by assuming the diffusion coefficient as a function of turbulent

viscosity of the respective phase. This helps avoid instantaneous solution instability due to cavitation.

For more information about this treatment, see Diffusion in VOF Model in the Fluent Theory Guide.

The generalized turbulent diffusion treatment can be used for simulating flows with two or more

phases. By default, for a flow with more than two phases, the turbulent diffusion acts between

primary and secondary phases only. The turbulent diffusion between secondary phases is not accoun-

ted for.

If you want to use the old turbulent diffusion treatment supported in releases prior to Release .,

enter the following text commands:

solve/set/multiphase-numerics/heat-mass-transfer/cavitation/turbulent-

diffusion

use generalized treatment of turbulent diffusion [yes] no

diffusion

use old treatment of turbulent diffusion [yes] yes

Unlike the generalized turbulent diffusion treatment, the old treatment is applicable to only two-

phase flows. If used for flows with more than two phases, the old treatment unphysically accounts

for each secondary phase interacting with the primary phase, despite the secondary non-vapor

phases not participating in cavitation.

If your want to disable the turbulent diffusion treatment for cases where the high turbulent viscosity

may be a source of an unstable solution, enter the following text commands:

diffusion

use old treatment of turbulent diffusion [yes] no

The evaporation-condensation mass transfer mechanism enables you to apply the evaporation-

condensation model as the mass transfer mechanism. The VOF and Mixture multiphase models use

the Lee model (see Lee Model in the Fluent Theory Guide). With the Eulerian multiphase model, you

can choose between the Lee model and the Thermal Phase Change model (see Thermal Phase

Change Model in the Fluent Theory Guide). When you select evaporation-condensation under

Mechanism in the Phase Interactions dialog box (Mass tab), you will be prompted with the

Evaporation-Condensation Model dialog box. Note that this dialog box could also be accessed by

clicking Edit... next to the evaporation-condensation mechanism drop-down list.

Figure . : The Evaporation-Condensation Model Dialog Box (Eulerian Multiphase Model)

You need to specify the following settings:

. (Eulerian multiphase model only) Select the evaporation-condensation Model.The following models

Lee

Thermal Phase Change

. Specify the Saturation Temperature for your flow regime. In addition to the methods described in

Defining Properties Using Temperature-Dependent Functions (p. ) (constant, polynomial, piecewise-

linear, piecewise-polynomial, or user-defined) you can choose one of the following:

tabular-pt-sat

The tabular-pt-sat allows you to specify saturation temperature using a table that contains

data points for saturation temperature and saturation pressure. Saturation temperature will

be interpolated based on the absolute pressure from the solution, which is assumed to be at

a saturated state. The table format is described in Specifying Variables in a Tabular

Format (p. ). Once you select tabular-pt-sat, the Table Input dialog box opens where you

can select the appropriate table and the names of the columns for your simulation from the

Saturation Temperature and Saturation Pressure selection lists.

tabular-ptl-sat

(available only with Alternative Modeling of Energy Sources (p. )) The method allows you

to specify saturation temperature using a table that contains data points for saturation tem-

perature, saturation pressure, and latent heat. Saturation temperature and latent heat will be

interpolated based on absolute pressure from the solution, which is assumed to be at a saturated

state. The table format is described in Specifying Variables in a Tabular Format (p. ). Once

you select tabular-ptl-sat, the Table Input dialog box opens where you can select the appro-

priate table and the names of the columns from the Saturation Temperature, Saturation

Pressure and Latent Heat selection lists.

Note

If you use tabular-pt-sat or tabular-ptl-sat to specify saturation temperature, you must

first read an appropriate table following the procedure outlined in Specifying Variables

in a Tabular Format (p. ). All table data must be in SI units (saturation temperature in

Kelvin (K), saturation pressure in Pascal (Pa), and latent heat in Joule/Kg).

If you use the tabular-pt-sat, tabular-ptl-sat, polynomial, piecewise-polynomial, or

piecewise-linear option for Saturation Temperature, the pressure-dependency must

be specified in terms of absolute pressure.

. (Lee model only) Specify the Evaporation Frequency and Condensation Frequency model constants.

These values correspond to the coefficient

(Equation . in the Theory Guide).The values

are . by default. However, note that the bubble diameter and accommodation coefficient are usually

not very well known, so the appropriate values for a given problem can be very different. It is important

to tune the values to match experimental data.

. (Mixture multiphase model only) For certain models and conditions, you can select the Semi-Mechan-

istic boiling model to model sub-cooled nucleate boiling at low pressure, as described in Including

Semi-Mechanistic Boiling (p. ).

. (Thermal Phase Change model only) Specify the following model coefficients:

From Phase Scaling Factor:

To Phase Scaling Factor:

If you are using the two-resistance option for heat transfer, these values act as multipliers for

the phase heat transfer coefficients determined for each phase and the default value of  is

usually appropriate. If you are using one of the other heat transfer options, then these parameters

correspond to the coefficient

(Equation . in the Theory Guide) and should be tuned

based on experimental data.

Note

For a phase pair, only one evaporation-condensation mechanism that uses the Thermal

Phase Change model can be defined, and it cannot be combined with other mass

transfer mechanisms.

The species-mass-transfer mechanism enables you to model generalized interphase species mass

transfer in either the Mixture model or the Eulerian model subject to the following conditions:

Both phases consist of mixtures with at least two species, and at least one of species is present in both

phases.

The two mixture phases are in contact and separated by an interface.

Species mass transfer can only occur between the same species from one phase to the other. For example,

evaporation/condensation between water liquid and water vapor.

As in all interphase mass transfer models in Fluent, if a gas mixture is involved in an interphase species

mass transfer process, it is always treated as a To Phase and the liquid mixture as a From Phase.

For the species involved in the mass transfer, the mass fractions in both phases must be determined by

solving transport equations. For example, the mass fractions of water liquid and water vapor in an

evaporation/condensation case must be solved directly from the governing equations, rather than algeb-

raically or from the physical constraint relations.

When you select species-mass-transfer under Mechanism in the Phase Interactions dialog box,

you will be prompted with the Species Mass Transfer Model dialog box.

Note

If multiple phase pairs have the species-mass-transfer mechanism selected, the same

settings in the Species Mass Transfer Model dialog box will be used for all phase pairs.

Figure . : The Species Mass Transfer Model Dialog Box

The steps to configure the species mass transfer model are as follows:

.

Under Model Options, choose the sub-model for determining the dynamic equilibrium relations

between the same species in a pair of phases.

Raoult’s Law

Use Raoult’s Law as described in Raoult’s Law in the Fluent Theory Guide.This model is appropriate

for gas-liquid cases in which the liquid phase can be modeled as an ideal liquid mixture. If you use

Raoult’s Law, you must specify the saturation pressure as a constant, polynomial, piecewise-linear,

piece-wise polynomial, or as a user-defined function using the DEFINE_PROPERTY macro.

Henry’s Law

Use Henry’s Law as described in Henry’s Law in the Fluent Theory Guide.This model is appropriate

for cases in which a gas species is dissolved into a liquid mixture phase. If you use Henry’s Law you

must specify the method for the Molar Fraction or Molar Concentration.You can choose a con-

stant, vant-hoff (to use the Van’t Hoff correlation), or a user-defined function using the

DEFINE_MASS_TRANSFER macro. For the vant-hoff model, you will need to specify Reference

Henry Constant (

in Equation . in the Fluent Theory Guide) and Temperature Dependence

(

) in the Vant Hoff’s Correlation dialog box.

Equilibrium Ratio

Use the Equilibrium Ratio method as described in Equilibrium Ratio in the Fluent Theory Guide.This

model allows you to specify the equilibrium ratio as a constant, or as a user-defined function. If

you use Equilibrium Ratio you must specify a constant or user-defined function using the

DEFINE_MASS_TRANSFER macro for Molar Fraction, Molar Concentration, or Mass Fraction.

.

Under Interphase Mass Transfer Coefficient, choose whether you want to specify the mass transfer

coefficient on a per-phase basis or on all phases:

If you selected Per Phase, you can choose the sub-models for calculating the phase-specific mass

transfer coefficients

and

for the source phase  and  the destination phase, respectively using

Equation . in the Fluent Theory Guide.The following models are available in ANSYS Fluent:

constant

Specify a constant value for the mass transfer coefficient.

sherwood-number

Specify a constant value for the Sherwood Number.The mass transfer coefficient is calculated

from Equation . in the Fluent Theory Guide.

ranz-marshall

Use the Ranz-Marshall model as described in Ranz-Marshall Model in the Fluent Theory Guide.

The Ranz-Marshall model is based on boundary layer theory for steady flow past a spherical

particle. It is applicable under the following flow conditions:

hughmark

hughmark

Use the Hughmark model as described in Hughmark Model in the Fluent Theory Guide.The

Hughmark model extends the Ranz-Marshall model for a wider range of relative Reynolds

number,

.

zero-resistance

Specify zero-resistance mass transfer between the bulk phase and interface.

Use a user-defined function for the mass transfer coefficient defined with the

DEFINE_MASS_TRANSFER macro.

The selection of physically correct mass transfer correlations is highly problem dependent.

In the case of mass transfer between a continuous phase and a dispersed phase of approxim-

ately spherical particles, the following should be adequate under most situations:

– ranz-marshall or hughmark for the continuous phase

– zero-resistance for the dispersed phase

Using zero-resistance for the dispersed phase implies that the mass transfer occurs very

quickly from the interface to the bulk of the dispersed phase. Consequently, the interface

concentration and bulk concentration in the dispersed phase are equal. This is usually valid

for droplet evaporation or gas absorption/dissolution in bubbles. If there exists significant

resistance to the mass transfer on the dispersed phase side, one of the other correlations

should be chosen for the dispersed phase.

If you select Overall, you can specify the Overall Mass Transfer Coefficient

in the Fluent Theory Guide either as a constant or as a user-defined function.These options are the

same as those for the Per Phase option.The Overall option is recommended only if the mass

transfer coefficient in each phase is unknown.

For more information about these options, see Mass Transfer Coefficient Models in the Fluent

The boiling mechanism applies the boiling model as the mass transfer mechanism. This model is

only available with the Eulerian multiphase model (when Boiling is enabled in the Multiphase

Model dialog box). For information about the inputs in Figure . : The Boiling Model Dialog

Box (p. ), refer to Including the Boiling Model (p. ).

The procedure for setting multiphase cell and boundary conditions is slightly different than for single-

phase models. You will need to set some conditions separately for individual phases, while other

conditions are shared by all phases (that is, the mixture), as described in Boundary and Cell Zone

Conditions for the Mixture and the Individual Phases (p. ).

.... Steps for Setting Boundary Conditions

Setup →

The steps you need to perform for each boundary are as follows:

. Select the boundary in the Zone list in the Boundary Conditions task page.

. Set the conditions for the mixture at this boundary, if necessary. (For information about which conditions

need to be set for the mixture, refer to Boundary and Cell Zone Conditions for the Mixture and the Indi-

vidual Phases (p. ).)

a.

In the Phase drop-down list, select mixture.

a.

b. If the current Type for this zone is correct, click Edit... to open the corresponding boundary condition

dialog box (for example, the Pressure Inlet dialog box); otherwise, choose the correct zone type in

the Type drop-down list, confirm the change (when prompted), and the corresponding dialog box

will open automatically.

c.

In the boundary condition dialog box for the selected zone type (for example, the Pressure Inlet

dialog box for the Eulerian model, shown in Figure . :The Pressure Inlet Dialog Box for a Mix-

ture (p. )), specify the mixture boundary conditions.

Figure . : The Pressure Inlet Dialog Box for a Mixture

Note that only those conditions that apply to all phases, as described in Boundary and Cell

Zone Conditions for the Mixture and the Individual Phases (p. ), will appear in this dialog

box.

For information about inputs related to the relevant boundary conditions, refer to the appro-

priate sections for those boundary conditions.

d. If you have enabled the Wall Adhesion option in the Phase Interaction dialog box (Surface Tension

tab), you need to specify the contact angle at the wall for each pair of phases as a constant (as shown

in Figure . :The Wall Dialog Box for a Mixture in a Multiphase Calculation with Wall Adhe-

sion (p. )) or a user-defined function (see the Fluent Customization Manual for more information).

Figure . : The Wall Dialog Box for a Mixture in a Multiphase Calculation with Wall

Adhesion

The contact angle (

in Figure . : Measuring the Contact Angle (p. )) is the angle

Adhesion

between the wall and the tangent to the interface at the wall, measured inside the phase listed

in the left column under Wall Adhesion in the Momentum tab of the Wall dialog box. For

example, if you are setting the contact angle between the oil and air phases in the Wall dialog

box shown in Figure . : The Wall Dialog Box for a Mixture in a Multiphase Calculation with

Wall Adhesion (p. ),

is measured inside the oil phase. For more information, refer to Wall

Adhesion in the Theory Guide.

Figure . : Measuring the Contact Angle

The default value for all pairs is  degrees, which is equivalent to no wall adhesion effects

(that is, the interface is normal to the adjacent wall). A contact angle of °, for example, cor-

responds to water creeping up the side of a container, as is common with water in a glass.

e. Define additional boundary conditions that are specific to the multiphase models.

i.

(VOF model) If you enabled the Jump Adhesion option in the Phase Interaction dialog box,

specify the contact angle at the porous jump for each pair of phases. If you enable the Jump

Adhesion option in the Phase Interaction dialog box, this option becomes visible at each of the

porous jump boundaries.You can enable or disable the Jump Adhesion option in the Porous

Jump dialog boxes and provide the inputs for the contact angle at the desired porous jump

boundary, as shown in Figure . :The Porous Jump Dialog Box Displaying Jump Adhesion (p. ).

Figure . : The Porous Jump Dialog Box Displaying Jump Adhesion

The contact angle

is the angle at the porous jump. To constrain the contact angle at

the porous jump based on porous or non-porous fluid zones, enable the Constrained Two-

Sided Adhesion option. Otherwise, if it is disabled, then the forced two-sided adhesion

treatment is in effect. For more detail, see Jump Adhesion.

f.

Click OK once you complete the boundary condition definition for the mixture.

. Set the conditions for each phase at this boundary, if necessary. (See Boundary and Cell Zone Conditions

for the Mixture and the Individual Phases (p. ) for information about which conditions need to be set

for the individual phases.)

a.

In the Phase drop-down list, select the phase (for example, water).

Important

Note that, when you select one of the individual phases (rather than the mixture),

only one type of zone appears in the Type drop-down list. It is not possible to assign

phase-specific zone types at a given boundary; the zone type is specified for the

mixture, and it applies to all of the individual phases.

b. Click Edit... to open the boundary condition dialog box for this phase (for example, the Pressure

Inlet dialog box, shown in Figure . :The Pressure Inlet Dialog Box for a Phase (p. )).

Figure . : The Pressure Inlet Dialog Box for a Phase

c.

Specify the boundary conditions for the phase. Note that only those conditions that apply to the in-

dividual phase, as described in Boundary and Cell Zone Conditions for the Mixture and the Individual

Phases (p. ), will appear in this dialog box.

d. (Secondary phase only) For the pressure outlet, exhaust fan or outlet vent boundary, you can specify

the volume fraction specification method as one of the following options:

Backflow Volume Fraction:You can define the backflow volume fraction as a constant, a profile

(see Profiles (p. )), or a user-defined function (see the Fluent Customization Manual).

Figure . : The Pressure Outlet Dialog Box for a Phase

From Neighboring Cell:This option does not require the specification of the backflow volume

fraction, and the volume fraction value is directly taken from the neighboring cells.

In the case of reverse flow at the pressure outlet boundary, sometimes it becomes tricky to

specify the correct values for the backflow volume fraction. Incorrect specification might

lead to instability, convergence issues and unphysical behavior. The backflow volume fraction

specification from the neighboring interior cells can be a good choice if information at the

pressure outlet boundary is not known.

e. Click OK once you complete the boundary condition definition for the phase.

.... Steps for Setting Cell Zone Conditions

Setup →

Figure . : The Cell Zone Conditions Task Page

The steps for specifying the mixture and individual phase cell zone conditions are listed below:

. Select the cell zone in the Zone list in the Cell Zone Conditions task page.

. If needed, set the cell zone conditions for the mixture. (For information about which conditions need to

be set for the mixture, refer to Boundary and Cell Zone Conditions for the Mixture and the Individual

Phases (p. ).)

a.

a.

b. Make sure that the selected Type is appropriate for this zone and click Edit....

c.

In the Fluid dialog box, set the cell zone conditions that are applicable to the mixture.

d. Define additional cell zone conditions that are specific to the multiphase models.

i.

If Zonal Discretization is enabled in the Interface Modeling Options dialog box, you can specify

the Compressive Scheme Slope Limiter in the Multiphase tab of the Fluid dialog box.The

setting of the slope limiter can be any value between  and , inclusive.Values of , , and  cor-

respond to first order upwind, second order upwind, and compressive discretization, respectively

with intermediate values resulting in a blended formulation. For more details about the slope

limiter, refer to The Compressive Scheme and Interface-Model-based Variants in the Fluent Theory

Guide.

. If required, set the conditions for each phase. (See Boundary and Cell Zone Conditions for the Mixture

and the Individual Phases (p. ) for information about which conditions need to be set for the individual

phases.)

a.

In the Phase drop-down list, select the phase (for example, water) and click Edit....

b. In the Fluid dialog box, set the cell zone conditions that are applicable to the individual phase.

For more information about inputs for cell zone conditions, see Fluid Conditions (p. ).

.... Boundary and Cell Zone Conditions for the Mixture and the Individual

Phases

The boundary conditions you need to specify for the mixture and for the individual phases will depend

on which multiphase model you are using.

Phases

Details for each model are provided in the following sections:

.....VOF Model

..... Mixture Model

..... Eulerian Model

If you are using the VOF model, the conditions you need to specify for each type of boundary zone

are listed below and summarized in Table . : Phase-Specific and Mixture Conditions for the VOF

Model (p. ).

For an inlet vent, intake fan, pressure inlet, or velocity inlet, there are no conditions to be specified for

the primary phase. For each secondary phase, you will need to set the volume fraction as a constant, a

profile (see Profiles (p. )), or a user-defined function (see the Fluent Customization Manual). All other

conditions are specified for the mixture.

For an exhaust fan, outlet vent, or pressure outlet, there are no conditions to be specified for the primary

phase. For each secondary phase, you will need to specify the volume fraction specification method as

either Backflow Volume Fraction or From Neighboring Cell (see step . in Steps for Setting Boundary

Conditions (p. )). All other conditions are specified for the mixture.

For a mass-flow inlet, you will need to set the mass flow rate, mass flux, or average mass flux for each

individual phase. All other conditions are specified for the mixture.

Important

Note that if you read a VOF case that was set up in a version of ANSYS Fluent prior to

., you will need to redefine the conditions at the mass-flow inlets.

For an axis, fan, outflow, periodic, porous jump, radiator, solid, symmetry, or wall zone, all conditions are

specified for the mixture.There are no conditions to be set for the individual phases.

For a wall zone, you can specify the contact angle for the mixture if the wall adhesion option is enabled.

For a fluid zone, mass sources are specified for the individual phases, and all other sources are specified

for the mixture.

– If the fluid zone is not porous, all other conditions are specified for the mixture.

– If the fluid zone is porous, you will enable the Porous Zone option in the Fluid dialog box for the

mixture.The porosity inputs (if relevant) are also specified for the mixture.The resistance coefficients

and direction vectors, however, are specified separately for each phase. See User Inputs for Porous

Media (p. ) for the mixture.

– If Open Channel Flow and/or Open Channel Wave BC is/are enabled in the Multiphase Model dialog

box, then the Numerical Beach option becomes available under the Multiphase tab of the Fluid

dialog box.To learn how to include numerical beach in your simulation, refer to Numerical Beach

Treatment for Open Channels (p. ).

See Cell Zone and Boundary Conditions (p. ) for details about the relevant conditions for each

type of boundary. Note that the pressure far-field boundary is not available with the VOF model.

Table . : Phase-Specific and Mixture Conditions for the VOF Model

Mixture

Secondary Phase

Primary Phase

Type

all others

volume fraction

nothing

inlet vent, intake fan, pressure

inlet, velocity inlet

all others

specification method

nothing

exhaust fan, outlet vent,

pressure outlet

all others

mass flow/flux

nothing

all others

nothing

all others

mass-flow inlet

all others

nothing

nothing

axis; fan; outflow; periodic;

porous jump; radiator; solid;

symmetry; wall

pressure far-field

porous zone;

porosity; all others

mass source; other

porous inputs

fluid

If you are using the mixture model, the conditions you need to specify for each type of boundary

zone are listed below and summarized in Table . : Phase-Specific and Mixture Conditions for the

Mixture Model (p. ).

either Backflow Volume Fraction or From Neighboring Cell (step  in Steps for Setting Boundary

Conditions (p. ). All other conditions are specified for the mixture.

For an inlet vent, intake fan, or pressure inlet, you will specify for the mixture which direction specification

method will be used at this boundary (Normal to Boundary or Direction Vector). If you select the Dir-

ection Vector specification method, you will specify the coordinate system (3D only) and flow-direction

components for the individual phases. For each secondary phase, you will need to set the volume fraction

(as described above). All other conditions are specified for the mixture.

Important

Note that if you read a mixture multiphase case that was set up in a version of ANSYS

Fluent previous to ., you will need to redefine the conditions at the mass-flow inlets.

For a velocity inlet, you will specify the velocity for the individual phases. For each secondary phase, you

will need to set the volume fraction (as described above). All other conditions are specified for the mixture.

specified for the mixture.There are no conditions to be set for the individual phases. Outflow boundary

conditions are not available for the cavitation model.

If the fluid zone is not porous, all other conditions are specified for the mixture.

If the fluid zone is porous, you will enable the Porous Zone option in the Fluid dialog box for

the mixture. The porosity inputs (if relevant) are also specified for the mixture. The resistance

coefficients and direction vectors, however, are specified separately for each phase. See User Inputs

for Porous Media (p. ) for details about these inputs. All other conditions are specified for the

mixture.

type of boundary. Note that the pressure far-field boundary is not available with the mixture model.

Table . : Phase-Specific and Mixture Conditions for the Mixture Model

Mixture

Type

all others

nothing

exhaust fan; outlet vent;

dir. spec. method;

all others

coord. system; flow

direction; volume fraction

direction

inlet vent; intake fan;

pressure inlet

all others

all others

velocity; volume fraction

velocity

velocity inlet

all others

nothing

nothing

axis; fan; outflow (n/a for

cavitation model); periodic;

Mixture

Type

mass source; other porous

inputs

fluid

If you are using the Eulerian model, the conditions you need to specify for each type of boundary

zone are listed below and summarized in

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (for Laminar Flow) (p. )

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Mixture Turbulence

Model) (p. )

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Dispersed Turbu-

lence Model) (p. )

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Per-Phase Turbu-

Note that the specification of turbulence parameters will depend on which of the three multiphase

turbulence models you are using, as indicated in

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Dispersed Turbulence

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Per-Phase Turbulence

See Turbulence Models in the Theory Guide and Modeling Turbulence (p. ) for more information

about multiphase turbulence models.

phase if you are modeling laminar flow or using the mixture turbulence model (the default multiphase

turbulence model), except for backflow total temperature if heat transfer is on.

For each secondary phase, you will need to specify the volume fraction specification method as

Conditions (p. ). If the phase is granular, you will also need to set its backflow granular temper-

ature. If heat transfer is on, you will also need to set the backflow total temperature.

If you are using the mixture turbulence model, you will need to specify the turbulence boundary

conditions for the mixture. If you are using the dispersed turbulence model, you will need to

specify them for the primary phase. If you are using the per-phase turbulence model, you will

need to specify them for the primary phase and for each secondary phase.

All other conditions are specified for the mixture.

components for the individual phases. If heat transfer is on, you will also need to set the total temperature

for the individual phases.

For each secondary phase, you will need to set the volume fraction (as described above). If the

phase is granular, you will also need to set its granular temperature.

individual phase.You will also need to specify the temperature of each phase, since the energy equations

are solved for each phase.

For mass-flow inlet boundary conditions, you can specify the slip velocity between phases. When

you select a mass-flow inlet boundary for the secondary phase, two options will be available for

the Slip Velocity Specification Method, as shown in Figure . : Mass-Flow Inlet Boundary

Condition Dialog Box (p. ) :

– Velocity Ratio

The value for the Velocity Ratio is the secondary phase to primary phase velocity ratio. By de-

fault, it is ., which means velocities are the same (no slip). By entering a ratio that is greater

than ., you are indicating a larger secondary phase velocity. Otherwise, you can enter a ratio

that is less than . to indicate a smaller secondary phase velocity.

– Volume Fraction

If you specify the volume fraction at an inlet, ANSYS Fluent will calculate the phase velocities.

Important

– If a secondary phase has zero mass flux (that is, the Eulerian model is used to run a single

phase case), neither Velocity Ratio nor Volume Fraction will affect the solution.

– The Velocity Ratio and Volume Fraction slip velocity methods cannot be mixed for different

secondary phases.That is, you should specify one or the other condition for all phases.

The volume fraction is basically the fraction of area covered by that phase.

Figure . : Mass-Flow Inlet Boundary Condition Dialog Box

For a velocity inlet, you will specify the velocity for the individual phases. If heat transfer is on, you will

also need to set the static temperature for the individual phases.

For an axis, outflow, degassing, periodic, solid, or symmetry zone, all conditions are specified for the

mixture.There are no conditions to be set for the individual phases.

For a wall zone, shear conditions are specified for the individual phases. All other conditions are specified

for the mixture, including thermal boundary conditions, if heat transfer is on.

For a fluid zone, all source terms and fixed values are specified for the individual phases, unless you are

using the mixture turbulence model or the dispersed turbulence model. If you are using the mixture

turbulence model, source terms and fixed values for turbulence are specified instead for the mixture. If

you are using the dispersed turbulence model, they are specified only for the primary phase.

Media (p. ) for details about these inputs. All other conditions are specified for the mixture.

type of boundary. Note that the pressure far-field, fan, porous jump, radiator, and mass-flow inlet

boundaries are not available with the Eulerian model.

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (for Laminar Flow)

Mixture

Type

all others

volume fraction specification

method; gran. temperature (tot.

temperature)

(tot. temperature)

exhaust fan; outlet

vent; pressure outlet

dir. spec.

method; all

others

coord. system; flow direction;

volume fraction; gran.

temperature (tot. temperature)

direction (tot.

all others

velocity; volume fraction; gran.

velocity (tot.

all others

mass flow rate/flux; velocity

ratio/volume fraction; gran.

temperature (temperature)

mass flow rate/flux

(temperature)

all others

nothing

nothing

axis; outflow;

degassing; periodic;

solid; symmetry

all others

shear condition

wall

pressure far-field; fan;

porous jump; radiator

porosity; all

all source terms; all fixed values;

other porous inputs

all source terms; all

fixed values; other

fluid

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Mixture

Turbulence Model)

Mixture

Type

all others

method; gran. temperature

all others

Type

all others

all others

all others

all others

all others

nothing

nothing

all others

wall

Mixture

Type

porous jump;

radiator

source terms for

turbulence; fixed

other source terms; other fixed

values; other porous inputs

other source terms;

other fixed values;

fluid

values for

turbulence; porous

zone; porosity; all

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Dispersed

Mixture

Type

all others

turb. parameters (tot.

dir. spec.

others

direction; turb. parameters;

all others

all others

velocity; turb. parameters

all others

mass flow rate/flux; turb.

parameters (temperature)

all others

nothing

nothing

all others

wall

pressure far-field;

fan; porous jump;

radiator

momentum and mass sources;

momentum and mass fixed

momentum, mass, turb.

sources; momentum, mass,

turb. fixed values; other

fluid

Table . : Phase-Specific and Mixture Conditions for the Eulerian Model (with the Per-Phase

Mixture

Type

all others

method; turb. parameters; gran.

dir. spec.

others

volume fraction; turb.

parameters; gran. temperature

direction; turb. parameters

inlet vent; intake

fan; pressure inlet

Mixture

Type

all others

velocity; volume fraction; turb.

all others

all others

mass flow rate/flux; tub.

all others

nothing

nothing

all others

wall

radiator

others

momentum, mass, turb. sources;

momentum, mass, turb. fixed

sources; momentum,

mass, turb. fixed values;

fluid

.... Steps for Copying Cell Zone and Boundary Conditions

The steps for copying cell zone and boundary conditions for a multiphase flow are slightly different

from those described in Copying Cell Zone and Boundary Conditions (p. ) for a single-phase flow.

The modified steps are listed below:

. In the Cell Zone Conditions or Boundary Conditions task page, click the Copy... button.This will open

the Copy Conditions dialog box.

. In the From Cell Zone or From Boundary Zone list, select the zone that has the conditions you want

to copy.

. In the Phase drop-down list, select the phase for which you want to copy the conditions (either mixture

or one of the individual phases).

Important

Note that copying the boundary conditions for one phase does not automatically result

in the boundary conditions for the other phases and the mixture being copied as well.

Important

You need to copy the conditions for each phase on each boundary of interest.

. Click Copy. ANSYS Fluent will set all of the selected phase’s (or mixture’s) boundary conditions on the

zones selected in the To Cell Zones or To Boundary Zones list to be the same as that phase’s conditions

on the zone selected in the From Cell Zone or From Boundary Zone list. (You cannot copy a subset of

the conditions, such as only the thermal conditions.)

See Copying Cell Zone and Boundary Conditions (p. ) for additional information about copying

boundary conditions, including limitations.

Once you have initialized the flow (as described in Initializing the Solution (p. )), you can define the

initial distribution of the phases. For a transient simulation, this distribution will serve as the initial

condition at

; for a steady-state simulation, setting an initial distribution can provide added stability

in the early stages of the calculation.

You can patch an initial volume fraction for each secondary phase using the Patch Dialog Box (p. ).

Patch...

If the region in which you want to patch the volume fraction is defined as a separate cell zone, you

can simply patch the value there. Otherwise, you can create a cell “register” that contains the appro-

priate cells and patch the value in the register. See Patching Values in Selected Cells (p. ) for details.

.... Options for Patching Volume Fraction

You have additional options for how the volume fraction is patched in a user-defined register. By

default the patching procedure will initialize all of the cells in the register with the specified volume

fraction, without any special treatment for cells that are intersected by the fluid-fluid interface.

Patch Reconstructed Interface

This option uses piecewise-linear interface reconstruction to identify the fluid-fluid interface and

patches the actual volume fraction field in the cells that intersect the interface.

Important

The Patch Reconstructed Interface algorithm requires that the register coordinates

in the Region Adaption dialog box be well-ordered. That is: X Min < X Max; Y

Min < Y Max; Z Min < Z Max. In particular, if you use the Select Points with

Mouse feature to specify the coordinates, be sure that this condition is met.

The Patch Reconstructed Interface will be applied only on the last register that

was defined, even if multiple registers are selected in the Patch dialog box.

Therefore, it is recommended that you create and patch registers one at a time.

Volumetric Smoothing

This option smooths the volume fraction field on-demand by taking the volumetric average over

the cell neighbors.This can help provide better solution stability at startup. After enabling Volumetric

Smoothing, you can click Smooth to apply the smoothing. Note that the smoothing is applied to

the volume fraction field for all phases in the full domain.The Smoothing Relaxation Factor controls

the degree of smoothing applied.You can specify a value between  (no smoothing) and  (max-

imum smoothing). For most cases, the default value is recommended. For fine meshes you may

choose to try a larger value to aid solution startup. However, excessively large values can have an

undesirable effect during the solution as interface sharpening discretization schemes may deteriorate

the initial field.

The Smooth command can be used at any time after the solution has been initialized. It can

therefore also be used after reading a data file for postprocessing. However, note that the

smoothed field will overwrite the original volume fraction field in this case. Also note that

you must select a secondary phase variable from the drop-down list in the Patch dialog box

to expose the Volumetric Smoothing option.

.. Setting Up the VOF Model

For background information about the VOF model and the limitations that apply, refer to Overview of

the VOF Model in the Theory Guide.

This section is organized as follows:

... Solving Steady-State VOF Problems

... Guidelines for Using the Multiphase Pseudo Transient Solver

... Including Coupled Level Set with the VOF Model

... Modeling Open Channel Flows

... Modeling Open Channel Wave Boundary Conditions

... Recommendations for Open Channel Initialization

... Numerical Beach Treatment for Open Channels

... Defining the Phases for the VOF Model

... Setting Time-Dependent Parameters for the Explicit Volume Fraction Formulation

... Modeling Solidification/Melting

... Using the VOF-to-DPM Model Transition for Dispersion of Liquid in Gas

For steady-state VOF problems, ANSYS Fluent automatically enables the Pseudo Transient solution

method along with the Coupled pressure-velocity coupling scheme for better stability and faster

convergence. For more information about pseudo transient solutions, see Performing Pseudo Transient

When using the Pseudo Transient solution method in multiphase applications, follow the guidelines

For the fixed (User-Specified) time step method, you must provide a suitable pseudo time step size to the

solver.You can use the Automatic time step method to estimate the pseudo time step size for the simulation.

This can be done by setting the Verbosity to  and simulating your case for a few iterations.The pseudo-

time step size will be printed in the Fluent console.

For the Automatic time step method, decreasing the Time Scale Factor to a lower value (about .) will

provide better solution stability.

Sometimes, for stiff flow problems, convergence may not be achieved when using the Automatic time

step method. In such cases, consider switching to the fixed (User-Specified) time step method instead.

For steady state problems, you should never evaluate convergence based on residuals alone.To better

judge convergence, you should also monitor appropriate field variables at a particular location until the

value stops changing.

The Coupled with Volume Fractions option is recommended for open channel flow applications.

When using the VOF formulation, you can couple the level set method with it to help overcome some

limitations that exist in the interface tracking method of the VOF model and the level set method. To

use the coupled level set method with VOF, perform the following:

. Open the Multiphase Model dialog box.

Setup →

Models →

Setting Up the VOF Model

. Under Model, enable Volume of Fluid.

. Under Coupled Level Set + VOF, enable Level Set (see Figure . : Multiphase Model Dialog Box for the

VOF Model (p. )).

. (optional) In some cases, spurious currents can arise from the application of the surface tension

force in the momentum equation. In these cases you can use the /define/models/mul-

tiphase/coupled-level-set text command to use a revised formulation of the surface

tension force that weights the force towards the heavier phase in the interface cells. You can choose

from none (the default), density-correction, and heaviside-correction.

After the Level Set option is enabled, proceed as you normally would when setting up the VOF

model (described in Setting Up the VOF Model (p. )). For theoretical information, refer to Coupled

Level-Set and VOF Model.

Note

When using the Level Set option, the recommended scheme is the geo-reconstruct

scheme (see The Geometric Reconstruction Scheme).

Important

The level set method is only suitable for two-phase flow regime, where two fluids are not

interpenetrating.

The level set model can only be used when the VOF model is turned on. No mass transfer

is allowed.

The level set method is not compatible with the dynamic mesh model.

Normally, zero flux of the level set function is set as the default for the boundary conditions. Due to

the geometrical re-initialization procedure at each time step, the boundary conditions shall not have

any significant effect on the results. For more information, see Re-initialization of the Level-set Function

via the Geometrical Method.

Using the VOF formulation, open channel flows can be modeled in ANSYS Fluent. To start using the

open channel flow boundary condition, perform the following:

. Enable Gravity and set the gravitational acceleration fields.

Gravity → On

. Enable the volume of fluid model.

a.

Open the Multiphase Model dialog box.

Setup →

Models →

b. Under Model, enable Volume of Fluid.

c.

Under Formulation, select either Implicit or Explicit.

. Under VOF Sub-Models, select Open Channel Flow.

Note

The default VOF formulation is set to Implicit after enabling the Open Channel Flow

option. This is done to allow the use of larger time step sizes for such applications.

In order to set specific parameters for a particular boundary for open channel flows, enable the Open

Channel option in the Multiphase tab of the corresponding boundary condition dialog box.

Table . : Open Channel Boundary Parameters for the VOF Model (p. ) summarizes the types of

boundaries available to the open channel flow boundary condition, and the additional parameters

needed to model open channel flow. For more information on setting boundary condition parameters,

see Cell Zone and Boundary Conditions (p. ).

Table . : Open Channel Boundary Parameters for the VOF Model

Parameter

Parameter

Boundary Type

Inlet Group ID; Secondary Phase for Inlet; Flow Specification Method; Free Surface

Level, Bottom Level; Velocity Magnitude

Outlet Group ID; Pressure Specification Method; Free Surface Level; Bottom Level

Inlet Group ID; Secondary Phase for Inlet; Free Surface Level; Bottom Level; Mass

Flow Rates for the Phases

Secondary Phase for Inlet; Free Surface Level, Averaged Velocity Inputs/Segregated

Velocity Inputs (Available with Open Channel Wave Boundary Condition)

Flow Rate Weighting

outflow

Further details are provided in the following sections:

.... Defining Inlet Groups

.... Defining Outlet Groups

.... Setting the Inlet Group

.... Setting the Outlet Group

.... Determining the Free Surface Level

.... Determining the Bottom Level

.... Specifying the Total Height

.... Determining the Velocity Magnitude

.... Determining the Secondary Phase for the Inlet

.... Determining the Secondary Phase for the Outlet

.... Choosing the Pressure Specification Method

.... Choosing the Density Interpolation Method

.... Open Channel Flow Compatibility with Velocity Inlet

.... Recommendations for Setting Up an Open Channel Flow Problem

Open channel systems involve the flowing fluid (the secondary phase) and the fluid above it (the

primary phase).

If both phases enter through the separate inlets (for example, inlet-phase2 and inlet-phase1),

these two inlets form an inlet group. This inlet group is recognized by the parameter Inlet Group ID,

which will be same for both the inlets that make up the inlet group. On the other hand, if both the

phases enter through the same inlet (for example, inlet-combined), then the inlet itself represents

the inlet group.

Important

In three-phase flows, only one secondary phase is allowed to pass through one inlet group.

Outlet-groups can be defined in the same manner as the inlet groups.

Important

In three-phase flows, the outlet should represent the outlet group, that is, separate outlets

for each phase are not recommended in three-phase flows.

For pressure inlets and mass-flow inlets, the Inlet Group ID is used to identify the different inlets

that are part of the same inlet group. For instance, when both phases enter through the same inlet

(single face zone), then those phases are part of one inlet group and you would set the Inlet Group

ID to  for that inlet (or inlet group).

In the case where the same inlet group has separate inlets (different face zones) for each phase, then

the Inlet Group ID will be the same for each inlet of that group.

When specifying the inlet group, use the following guidelines:

Since the Inlet Group ID is used to identify the inlets of the same inlet group, general information such

as Free Surface Level, Bottom Level, or the mass flow rate for each phase should be the same for each

inlet of the same inlet group.

You should specify a different Inlet Group ID for each distinct inlet group.

For example, consider the case of two inlet groups for a particular problem. The first inlet group

consists of water and air entering through the same inlet (a single face zone). In this case, you

would specify an inlet group ID of  for that inlet (or inlet group). The second inlet group consists

of oil and air entering through the same inlet group, but each uses a different inlet (oil-inlet

and air-inlet) for each phase. In this case, you would specify the same Inlet Group ID of  for

both of the inlets that belong to the inlet group.

For pressure outlet boundaries, the Outlet Group ID is used to identify the different outlets that are

part of the same outlet group. For instance, when both phases enter through the same outlet (single

face zone), then those phases are part of one outlet group and you would set the Outlet Group ID

to  for that outlet (or outlet group).

In the case where the same outlet group has separate outlets (different face zones) for each phase,

then the Outlet Group ID will be the same for each outlet of that group.

When specifying the outlet group, use the following guidelines:

Since the Outlet Group ID is used to identify the outlets of the same outlet group, general information

such as Free Surface Level or Bottom Level should be the same for each outlet of the same outlet group.

You should specify a different Outlet Group ID for each distinct outlet group.

For example, consider the case of two outlet groups for a particular problem. The first outlet group

consists of water and air exiting from the same outlet (a single face zone). In this case, you would

specify an outlet number of  for that outlet (or outlet group). The second outlet group consists

of oil and air exiting through the same outlet group, but each uses a different outlet (oil-outlet

and air-outlet) for each phase. In this case, you would specify the same Outlet Group ID of

for both of the outlets that belong to the outlet group.

Important

For three-phase flows, when all the phases are leaving through the same outlet, the outlet

should consist only of a single face zone.

For the appropriate boundary, you need to specify the Free Surface Level value. This parameter is

available for all relevant boundaries, including pressure outlet, mass-flow inlet, and pressure inlet.

The Free Surface Level, is represented by

(.)

where  is the position vector of any point on the free surface, and  is the unit vector in the direction

of the force of gravity. Here a horizontal free surface that is normal to the direction of gravity is as-

sumed.

We can simply calculate the free surface level in two steps:

. Determine the absolute value of height from the free surface to the origin in the direction of gravity.

. Apply the correct sign based on whether the free surface level is above or below the origin.

If the liquid’s free surface level lies above the origin, then the Free Surface Level is positive (see

Figure . : Determining the Free Surface Level and the Bottom Level (p. )). Likewise, if the liquid’s

free surface level lies below the origin, then the Free Surface Level is negative.

You can also specify a transient profiles for a Free Surface Level for the relevant open channel

boundaries as shown in the example below:

/*********************************************************************

Example UDF that demonstrates transient profile for free surface level

**********************************************************************/

#define H . /* Original Free surface level */

#define T0 . /* Time */

DEFINE_TRANSIENT_PROFILE(fs_level, current_time)

{

real level;

if (current_time <= T0)

level = H - current_time;

else

level = H - T0;

return level;

}

For the appropriate boundary, you need to specify the Bottom Level value. This parameter is available

for all relevant boundaries, including pressure outlet, mass-flow inlet, and pressure inlet. The Bottom

Level, is represented by a relation similar to Equation . in the Theory Guide.

(.)

where  is the position vector of any point on the bottom of the channel, and  is the unit vector

of gravity. Here we assume a horizontal free surface that is normal to the direction of gravity.

We can simply calculate the bottom level in two steps:

. Determine the absolute value of depth from the bottom level to the origin in the direction of gravity.

. Apply the correct sign based on whether the bottom level is above or below the origin.

If the channel’s bottom lies above the origin, then the Bottom Level is positive (see Figure . : De-

termining the Free Surface Level and the Bottom Level (p. )). Likewise, if the channel’s bottom lies

below the origin, then the Bottom Level is negative.

Figure . : Determining the Free Surface Level and the Bottom Level

You can also specify a transient profiles for a Bottom Level for the relevant open channel boundaries.

The total height, along with the velocity, is used as an option for describing the flow. The total height

is given as

(.)

where

is the velocity magnitude and  is the gravity magnitude.

For pressure inlet boundaries, input for Velocity Magnitude is required to calculate the dynamic

pressure being used in the total pressure calculation.

Note

The provided Velocity Magnitude is not applied to the boundary.

In the case of a flow with more than two phases, for pressure inlets and mass-flow inlets, you can

select the desired secondary phase from the Secondary Phase for Inlet drop-down box.

Important

Note that only one secondary phase is allowed to pass through one inlet group.

Consider a problem involving a three-phase flow consisting of air as the primary phase, and oil and

water as the secondary phases. Consider also that there are two inlet groups:

water and air

oil and air

For the former inlet group, you would choose water as the secondary phase. For the latter inlet group,

you would choose oil as the secondary phase (as shown in Figure . : Pressure Inlet for Open

Channel Flow (p. )).

Figure . : Pressure Inlet for Open Channel Flow

For a flow application with more than two phases, if you select Free Surface Level for the Pressure

Specification Method (in the Pressure Outlet dialog box, Multiphase tab), you must also select the

appropriate Secondary Phase for Level Specification and specify the Free Surface Level and Bottom

Level. See Determining the Free Surface Level (p. ) and Determining the Bottom Level (p. ) for

details about these parameters. For more information about the available pressure specification

methods, refer to Pressure Outlet in the Fluent Theory Guide.

The hydrostatic pressure profile is imposed in the selected secondary phase that shares the interface

with the primary phase. It is assumed that other secondary phases will not disturb the imposed

pressure distribution.

For example, in a three-phase cavitating flow consisting of air, water, and vapor, the vapor is generated

in the localized region adjacent to moving bodies. If the pressure outlet boundary is sufficiently far

away from the cavitating region, then the hydrostatic assumption in the water phase that shares the

interface with air can be safely imposed.

For a pressure outlet boundary, the outlet pressure can be specified in one of three ways:

by prescribing the free surface level, such as a hydrostatic pressure profile (available for two-phase flow

only)

by specifying the constant pressure

by specifying the neighboring cell pressure

Note

You can also specify a hydrostatic pressure profile at the pressure outlet for axisym-

Note

metric open channel flow. However, there are certain limitations as noted in Limita-

Important

This option is not available in the case of three-phase flows since the pressure on the

boundary is taken from the neighboring cell.

For problems involving sub-critical flow, the following options exist for the Density Interpolation

Method:

From Neighboring Cell is the default option, where the mixture density used in the hydrostatic profile

is interpolated using the volume fraction calculated from the neighboring cell.

Note

In some cases, this method may cause free surface oscillation near the upstream

boundaries. These oscillations are particularly visible in cases where boundaries are close

to the object; or if the boundary has unstructured mesh near the free surface level. For

such cases, it is recommended that you use the From Free Surface Level option under

Density Interpolation Method.

From Free Surface Level where the mixture density used in the hydrostatic profile is interpolated from

the volume fraction calculated from the free surface level.

Hybrid where the mixture density used in the hydrostatic profile is calculated either from the From

Neighboring Cell or From Free Surface Level options, depending on the direction of flux.This method

is only available at a pressure outlet.

Figure . : Density Interpolation Method for Open Channel Flow

.....Velocity Inlet, Open Channel Flow, Steady-State

.....Velocity Inlet, Open Channel Flow,Transient

Open channel flow compatibility with velocity inlet is provided in the framework of the open channel

wave boundary condition, therefore, the Open Channel Wave BC option in the Figure . : Multiphase

Model Dialog Box for the VOF Model (p. ) must be enabled first.

Velocity inlet compatibility allows you to use either averaged or segregated velocity inputs to moving

obstacles, water and air, which is not possible using either the pressure inlet or mass-flow inlet

boundary conditions.

Select the Open Channel Wave BC option in the Velocity Inlet dialog box. For detailed information

about the velocity inputs, see Inputs at Velocity Inlet Boundaries (p. ).

you must specify (in the Multiphase tab of the Velocity Inlet dialog box):

Secondary phase for the inlet

Free surface level

You must set the Wave BC Option to None (in the Multiphase tab of the Velocity Inlet dialog

box).

The following list summarizes some issues and limitations associated with the open channel boundary

The conservation of the Bernoulli integral does not provide the conservation of mass flow rate for the

pressure boundary. In the case of a coarser mesh, there can be a significant difference in mass flow rate

from the actual mass flow rate. For finer meshes, the mass flow rate comes closer to the actual value. So,

for problems having constant mass flow rate, the mass flow rate boundary condition is a better option.

The pressure boundary should be selected when steady and non-oscillating drag is the main objective.

Specifying the top boundary as the pressure outlet can sometimes lead to a divergent solution.This may

be due to the corner singularity at the pressure boundary in the air region or due to the inability to specify

local flow direction correctly if the air enters through the top locally.

Only the heavier phase should be selected as the secondary phase.

In the case of flows with more than two phases, only one secondary phase is allowed to enter through

one inlet group (that is, the mixed inflow of different secondary phases is not allowed).

For axisymmetric flow, pressure and mass-flow inlets do not support open channel boundary conditions.

Open channel wave boundary conditions for velocity inlets do not support cases with axisymmetric flow.

Axisymmetric open channel flow is available for two phase flow and the pressure outlet boundary.

For axisymmetric open channel flow, the direction of gravity must be aligned with the direction of the

axis.

The following list represents a list of recommendations for solving problems using the open channel

flow boundary condition:

In the cases where the inlet group has a different inlet for each phase of fluid, then the parameter values

(such as Free Surface Level, Bottom Level, and Mass Flow Rate) for each inlet should correspond to all

other inlets that belong to the inlet group.

The solution begins with an estimated pressure profile at the outlet boundary.

In general, you can start the solution by assuming that the level of liquid at the outlet corresponds

to the level of liquid at the inlet. The convergence and solution time is very dependent on the initial

conditions. When the flow is completely subcritical (upstream and downstream), in marine applic-

ations for instance, the above approach is recommended.

If the final conditions of the flow can be predicted by other means, the solution time can be signi-

ficantly reduced by using the proper boundary condition.

In the case of super-critical flow at the outlet, you can use the From Neighboring Cell option at the outlet,

as it may provide better convergence.

The initialization procedure is very critical in the open channel analysis. Refer to Recommendations for

Open Channel Initialization (p. ).

For the initial stability of the solution, a smaller time step is recommended.You can increase the time step

once the solution becomes more stable.

For flows that do not make a transition from sub-critical to super-critical, or vice-versa, you can speed-up

the solution calculation by specifying the frequency of Froude number updates during run time by setting

the following text command: solve → set → open-channel-controls.

When prompted, set up the following parameter for steady-state flows:

/solve/set> open-channel-controls

Iteration interval for Froude number update []

When prompted, set up the following parameter for transient flows:

Time step interval for Froude number update []

For pure open channel flow applications, the inlet and outlet boundary conditions are controlled by the

Froude number. In certain cases, it is possible to impose a hydrostatic profile at the outlet without any

Froude number dependency.You can use the following text command: solve → set → open-channel-

controls.

When prompted, set up the following parameter as shown below:

Use Froude number independent boundary condition at outlet? [no] yes

Relevant open channel inputs, along with the Froude number, can be reported using the following text

command: define → boundary-conditions → openchannel-threads.

In the case of reverse flow, the pressure outlet boundary behaves as a pressure inlet, and the boundary-

specific static pressure is taken as the Total Pressure. In this case, the static pressure is calculated from

the total pressure.You can use the following text command to fix the boundary-specified static pressure,

which helps to suppress reflections from the pressure boundary for certain cases: solve → set → open-

channel-controls

Use boundary specified static pressure for backflow? [no] yes

When modeling open channel wave boundary conditions, many of the variables that are used in open

channel flow, also exist for open channel wave boundary conditions. You may have to refer to Modeling

Open Channel Flows (p. ) for information about some of the settings.

To use the open channel wave boundary condition, perform the following:

. Enable the Volume of Fluid model in the Multiphase Model dialog box.

Setup →

Models →

. Under Formulation, select either Implicit or Explicit.

. Under VOF Sub-Models, select Open Channel Wave BC.

In order to set specific parameters for a particular boundary for open channel wave boundaries, enable

the Open Channel Wave BC option in the Velocity Inlet boundary condition dialog box (Fig-

ure . : The Velocity Inlet for Open Channel Wave BC (p. )).

Figure . : The Velocity Inlet for Open Channel Wave BC

The default method is the Averaged Flow Specification Method, where inputs for the moving obstacle

and water current are combined. There is no specific treatment for air velocity, which is assumed to

be same as the averaged velocity.

Segregated Velocity Inputs

The Segregated Velocity Inputs option allows you to prescribe velocity inputs individually for the

moving obstacle, Secondary phase (typically water), and Primary phase (typically air).

Figure . : Segregated Velocity Inputs for Open Channel Wave BC

You can set the moving object and secondary phase velocity specification methods as:

Magnitude and direction vector

Magnitude and normal to boundary

You can set the primary phase velocity specification methods as:

Power law and direction vector

Power law and normal to boundary

Power Law

(.)

Where

is the vertical distance from the instantaneous free surface level at which the reference

velocity magnitude,

is specified.

is the vertical distance from the free surface level at which,

velocity

must be estimated.

is the power law coefficient, which is typically . for an open

sea.

Setting Buffer Layer Height

The buffer layer is assumed to be the layer above the free surface, in which the effect of air is not felt.

This option is provided by assuming that the air in the vicinity of free surface blows with the speed of the

water and the waves, so that direct effect of air is not felt in the wave propagation.

There are two options for providing the buffer height:

.

Automatic: the buffer layer is taken as the specified fraction of the maximum wave height.

.

User-defined: you provide the input for the buffer layer height.

The buffer layer can also be defined using the following text command:

/solve/set> open-channel-wave-options

/solve/set/open-channel-wave-options>

set-buffer-layer-ht     set-verbosity           stokes-wave-variants

/solve/set/open-channel-wave-options> set-buffer-layer-ht

buffer layer specification method ( - Automatic,  - User-defined)  []

fraction of buffer layer height to maximum wave height [.]

enter the value of buffer layer height []

In the Momentum tab of the Velocity Inlet dialog box, you can enter the averaged flow velocity,

which includes components from the flow current and the moving object. You can specify the Averaged

Flow Specification Method as:

Magnitude and Direction

Magnitude and Normal to Boundary

Components

In the Multiphase tab (Figure . : The Velocity Inlet for Open Channel Wave BC (Explicit Formula-

tion) (p. )), you will specify the following:

Figure . : The Velocity Inlet for Open Channel Wave BC (Explicit Formulation)

Secondary Phase for Inlet specifies the phase to which the wave parameters are applied. In case of a

three-phase flow, select the corresponding secondary phase from this list.

Wave BC Options of which you have a choice of Shallow/Intermediate Waves, Short Gravity Waves,

Shallow Waves, and None (for calm sea or pure open channel flow problems without waves). Information

about these waves is available in Open Channel Wave Boundary Conditions in the Theory Guide. Note that

the short gravity waves expression is derived under the assumption of infinite liquid height.

Free Surface Level is the same definition as for open channel flow, see Modeling Open Channel

Flows (p. ).

Bottom Level is the same definition as for open channel flow, see Modeling Open Channel Flows (p. ),

and is valid only for shallow or intermediate depth waves.The bottom level is used for calculating the liquid

height.

Reference Wave Direction is the direction of wave propagation with zero wave heading angle.You can

specify the wave propagation direction as:

– Averaged Flow Direction: In this case, the reference direction is the same as the averaged flow direction.

– Direction Vector

– Normal to Boundary

Wave Modeling Options determines how the waves are modeled in the shallow/intermediate and short

gravity wave regimes.You can choose to model the waves using either Wave Theories or Wave Spectrum.

Wave Theories is usually selected for simulating regular waves.To simulate random waves, select Wave

Spectrum.

Depending on your choice of Wave BC Options and Wave Modeling Options, you will need to specify

the wave parameters as described in the following sections.

Shallow Wave Inputs (p. )

Wave Group Inputs (p. )

Wave Spectrum Inputs (p. )

Shallow Wave Inputs

If you have selected Shallow Waves for Wave BC Options you can specify the following settings for

each wave:

Number of Waves

is the option to set the number of interacting waves (default = )

Ideally, shallow waves do not support the principle of superposition. The Number of Waves option

enables interaction of two different waves originating at unique (non-interfering) locations within

the domain. Collision of two counter-propagating solitary waves inside a domain is an example of

a shallow wave interaction.

Wave Theory

of which you have a choice of Fifth Order Solitary (the default) and Fifth Order Cnoidal. Information

about the types of wave theory is available in Open Channel Wave Boundary Conditions in the Theory

Guide.

Wave Height

is the height difference between a wave crest to the neighboring trough.

Since a solitary wave does not have troughs, the wave height is the distance between a wave crest

to mean free surface level.

Wave Length

is the distance between two consecutive zero crossings.

Since solitary waves are derived based on the assumption of infinite wave length, specified wave

length is only used to estimate the elliptic function parameter for suitability of the wave theory,

and is not used in calculating wave parameters.

Inlet Offset Distance

is the translational distance from the reference point origin in the reference wave propagation direction.

This option is used to generate a wave from a location other than the reference frame origin. For a solitary

wave, the hump is always generated at the location where:

(.)

where  and

are spatial coordinates in the reference wave propagation direction.

Wave Heading Angle

is the angle between the direction of the wavefront and the reference wave propagation direction, in the

plane of the flow surface. In 2D, there are only two possibilities, zero degree when the wave is in the ref-

erence propagation direction, and  degree when the wave Is in the direction opposite to the reference

propagation direction.

Wave Group Inputs

If you have selected Wave Theories for Wave Modeling Options you can specify the following settings

for each wave:

is the option to set the number of superposed waves (default = )

of which you have a choice of First Order Airy (the default), Second Order Stokes, Third Order Stokes,

Fourth Order Stokes, and Fifth Order Stokes. Information about the types of wave theory is available

in Open Channel Wave Boundary Conditions in the Theory Guide.

is the distance between two consecutive crests, troughs or zero crossings.

Phase Difference

is the phase angle by which one periodic disturbance or wavefront lags behind or precedes another in

time or space.

Wave Spectrum Inputs

If you have selected Wave Spectrum for Wave Modeling Options you can specify the following settings

Frequency Spectrum Method

specifies the spectrum to use.You can select Pierson-Moskowitz (appropriate for fully-developed seas),

Jonswap (appropriate for fetch-limited seas), or TMA (appropriate for fetch-limited, finite-depth seas).

Peak Shape Parameter

controls the shape and amplitude of the frequency peak in the Jonswap and TMA formulations.This

corresponds to  in Equation . in the Fluent Theory Guide.

Significant Wave Height

is the mean wave height of the largest / of waves.This corresponds to

Peak Wave Frequency

is the wave frequency corresponding to the highest wave energy.This corresponds to

and Equation . in the Fluent Theory Guide.

can be expressed in terms of the peak wave period,

, as

.

, as

.

Minimum/Maximum Wave Frequency

specify the frequency range for the spectrum. Note that the Peak Wave Frequency must fall in between

Minimum Wave Frequency and Maximum Wave Frequency.

Number of Frequency Components

specifies the number of components into which the frequency spectrum is divided.

Direction Spreading Method

specifies the method to use for specifying the directional spreading characteristics.You can choose Uni-

directional (for long-crested waves), Frequency Independent Cosine Function (for short-crested waves

where the directional component does not depend on frequency), and Frequency Dependant Hyper-

bolic Function (for short-crested waves where the directional component depends on frequency).

Frequency Independent Cosine Exponent

specifies the exponent in the Frequency Independent Cosine Function formulation.This corresponds to

Mean Wave Heading Angle

specifies the principal wave heading direction.

Angular Spread

specifies the deviation from the mean wave direction for calculating the angular range.

Number of Angular Components

specifies the number of components into which the angular range is divided.

The total number of wave components is the product of Number of Frequency Components and

Number of Angular Components. For modeling random waves, phase differences for the individual

wave components are randomly distributed between  and 2π.

Note

Any change in the input for Number of Wave Components will change the values of

phase difference for each component. Therefore, it is recommended that you start the

Note

simulation from a saved case file after setting all the wave spectrum user inputs and

that you not change the number of wave components during the simulation.

.... Summary Report and Regime Check

A useful text command used to print out a summary of the open channel wave boundary condition

settings is define/boundary-conditions/open-channel-wave-settings. The output

will depend on whether you have chosen Wave Theories or Wave Spectrum.

Sample Output for Wave Theories

/define/boundary-conditions> open-channel-wave-settings

Wave Input Analysis for Velocity Inlet : Thread ID =

************************************************************

Wave- Analysis

*****************************************

Current Settings :

------------------

Wave theory : 5th-order-Stokes , Wave regime = Shallow/Intermediate

Wave Height (H) = ., Wave Length (L) = .

Liquid Depth (h) = ., Ursell Number (H*L*L/(h*h*h)) = .

Mandatory checks for full wave regime within wave breaking limit

-----------------------------------------------------------------

Relative Height: H/h = . , Maximum theoretical limit = .

Maximum numerical limit = .

Relative height within wave breaking limit

Wave Steepness: H/L = . , Maximum theoretical limit = .

Stable numerical limit = . , Maximum numerical limit = .

Warning: Wave steepness exceeding the stable numerical limit.

Waves could be stable or unstable in this regime.

Checks for selected wave theory within wave breaking and stability limit

----------------------------------------------------------------------------

Relative height check

H/h = . , Min : . , Max : .

Relative height check : successful

Wave Steepness check

H/L = . , Min : . , Max : .

Wave steepness check : successful

Ursell Number check

Ur = . , Min : . , Max : .

Ursell number check : successful

Wave regime check

h/L = . , Min : . , Max : .

Wave regime check : successful

Summary

----------------------

Checks : passed

Selected wave theory is appropriate for application.

Sample Output for Wave Spectrum

Wave Spectrum Analysis

Frequency Spectrum : Jonswap

Direction Spreading Method : Unidirectional

Significant Wave Height (Hs) = .

Peak Wave Frequency (wp) = ., Peak Time Period (Tp) = .

Minimum Frequency (wi) = ., Maximum Frequency (we) = .

Wave Lengths at Min/Peak/Max frequencies (Li, Lp, Le) = (., ., .)

Recommendation: Set the min and max wave frequencies so that most of the wave energy

is concentrated in the selected regime of spectrum.

Min frequency = . *Peak frequency

Max frequency = . *Peak frequency

Wave Regime Check

Wave regime type = Short Gravity (Deep)

Information: Validity of short gravity assumption : Liquid Depth > . *Max Wave Length

Sea Steepness Check

-----------------------

Peak Time Period (Tp) = .

Zero Upcrossing Time Period (Tz) = .

Sea Steepness based on Tp (Sp) = ., Steepness Limit = .

Sea Steepness based on Tz (Sz) = ., Steepness Limit = .

Warning: Sea Steepness based on peak time period exceeding limit.

Warning: Sea Steepness based on zero upcrossing time period exceeding limit.

Information: High wave steepness of any individual component too could affect the wave pattern,

as superposition of wave components is based upon lienar wave theory.

Frequency Spectrum Check

---------------------------

Peak Time Period to Wave Ht Sqrt Ratio (r = Tp/sqrt(Hs)) = .

Message: Selection of Jonswap spectrum is appropriate.

Recommended value of Peak Shape Parameter for r <= . :  .

Spectrum Resolution check

----------------------------

Number of frequency components =

Number of angular components =

Total number of wave components =

Information: Higher number of wave components would have adverse effect on speed-up

whereas smaller could affect the accuracy by not resolving the spectrum well.

Following steps could assist to optimize the number of components

. Set number of frequency/angular components in boundary condition panel,

. Set TUI command solve> set> open-channel-wave-verbosity to  before initialization,

. Initialize (It would print Spectrum Energy for each frequency/angle.)

. Copy the information to plot Sw vs Omega and S_theta vs theta

. Optimize the number of components after repeating steps -

....Transient Profile Support for Wave Inputs

ANSYS Fluent supports transient profiles for all wave inputs using user-defined functions as seen by

the example below:

/***********************************************************************

UDF for defining transient profile wave inputs

************************************************************************/

#include "udf..h"

#define H . /* wave height for both waves : same */

#define LEN1 . /* wave length for first wave */

#define LEN2 . /* wave length for second wave*/

#define G .

#define D . /* liquid depth */

#define U . /* wave current */

#define X . /* inlet point */

DEFINE_TRANSIENT_PROFILE(wave_ht, current_time)

{

real k1 = . *M_PI/LEN1;

real k2 = . *M_PI/LEN2;

real w1 = sqrt(G*k1*tanh(k1*D)) + k1*U;

real w2 = sqrt(G*k2*tanh(k2*D)) + k2*U;

real dk = . *(k1 - k2);

real dw = . *(w1 - w2);

return (. *H*cos(dk*X - dw*current_time));

}

.... Alternative Stokes Wave Theory Variant

Fluent uses Fenton’s formulation for Stokes theories by default. For additional information about the

current Stokes theories formulation, see Stokes Wave Theories in the Fluent Theory Guide. To revert

to the old formulation, provided by Skjebreia and Hendrickson, use the following text command:

/solve/set/open-channel-wave-options> stokes-wave-variants

Use Fenton's formulation for Stokes wave theories [yes] no

Activating old formulation (Skjelbreia and Hendrickson) for Stokes wave theories.

For additional information on the old formulation, refer to Lin’s book [] (p. ).

Once you have selected either the Open Channel Flow or the Open Channel Wave BC option in the

Multiphase Model dialog box, then the Open Channel Initialization Method drop-down list appears

in the Solution Initialization task page.

Solution →

Figure . : The Solution Initialization Task Page

Select an inlet zone from the Compute from drop-down list. You can now make your selection from

the Open Channel Initialization Method drop-down list. If only the Open Channel Flow option was

enabled, then you only have a choice of None or Flat. If you enabled Open Channel Wave BC, then

your choices are None, Flat, or Wavy. The default initialization method is None.

If you initialize the solution using None, it has no effect as it does not use any open channel information

from the selected zone. The Open Channel Initialization Method comes into effect when you select

either Flat or Wavy.

Important

This initialization is only valid for pressure-inlets, pressure outlets, and mass-flow inlets for

open channel flow and velocity inlets for open channel wave boundary conditions. If the

selected inlet zone does not have either open channel flow or open channel wave boundary

conditions, ANSYS Fluent will report an error message after you initialize the flow with open

channel initialization method of Flat or Wavy.

For open channel initialization from the pressure outlet boundary, the hydrostatic pressure profile

based on the Free Surface Level is patched in the domain. The volume fraction in the domain is

patched based on Free Surface Level provided at the pressure outlet boundary. To patch velocity

and other variables, the values in the Solution Initialization task page will be used.

Important

Important

The pressure specification methods, with the exception of Free Surface Level, are not

supported for open channel initialization from the pressure outlet boundary.

Initialization will result in the volume fraction, X, Y, and Z velocities, and pressure being patched in

the domain. The volume fraction will be patched in the domain based on the free surface level of the

selected zone from the Compute from list. The velocities in the domain will be patched assuming the

constant value provided for the velocity magnitude in the selected zone.

Important

If you specify a profile for the velocity magnitude or direction vectors, the initialization will

select the value for the velocity magnitude and direction vectors from only one face.

Therefore the initialization may be inaccurate. However, generally, open channel inputs for

velocity magnitude and direction vectors are constant.

The pressure that is patched is the hydrostatic pressure based on the free surface level specified in

the selected zone.

You can use the following text command for open channel automatic initialization:

solve → initialize → open-channel-auto-init

When prompted, set up the following parameters:

boundary thread id

Enter the thread id for the boundary to be selected for open channel automatic initialization.

flat free surface initialization

This option is available for both open channel flow and open channel wave boundary conditions.

wavy free surface initialization

This option appears only for open channel wave boundary conditions, when flat free surface initialization

is not selected.

The steps to be followed for open channel automatic initialization are

. Compute defaults based on valid open channel boundary thread.This step is required for better initializ-

ation of turbulence parameters based on uniform velocity magnitude.

solve → initialize → compute defaults

. This would provide information about the selected boundary and type of initialization.

. Initialize

solve → initialize → initialize

.... Reporting Parameters for Open Channel Wave BC Option

To report values as wave speed, wave frequency, and time period for individual waves during initial-

ization, you can set the following text command:

solve → set → open-channel-wave-options → set-verbosity

When prompted to set Verbosity for reporting of derived wave inputs during

initialization, enter  as shown below:

Note

You can enter values of , , or . Entering a higher number provides more information.

/solve/set/open-channel-wave-options> set-verbosity

Verbosity for reporting of derived wave inputs during initialization

[]

A sample of the resulting output for wave groups after initializing is shown below:

Wave- : Wave Height = ., Wave Length = .

Wave Number = ., Wave Speed = ., Wave Frequency = .

Effective parameters: Wave Speed = ., Wave Frequency = ., Time Period = .

Time Period based on average effective frequency: .

The resultant output for Shallow Waves option is shown below:

Wave- : Wave Height = ., Specified Wave Length = .

Wave Number = ., Estimated Wave Length = .

Elliptic Function Parameter (m) : Calculated = ., Used = .

Liquid Height = ., Trough Height = .

Wave Speed = ., Wave Frequency = .

Effective parameters: Wave Speed = ., Wave Frequency = .

Time Period based on effective frequency: .

In certain applications, it is desirable to suppress numerical reflection near the outlet boundary for

wave dampening. To understand the theory involved in this application, refer to Numerical Beach

Treatment.

To include numerical beach in your simulation, perform the following:

Setup →

Models →

. Under Scheme, select either Implicit or Explicit.

. Select Open Channel Flow and/or Open Channel Wave BC.

In order to set the numerical beach parameters for a fluid zone, go to the Fluid dialog box (Fig-

ure . : The Fluid Dialog Box to Enable Numerical Beach (p. )).

Figure . : The Fluid Dialog Box to Enable Numerical Beach

In the Multiphase tab of the Fluid dialog box, enable the Numerical Beach option and enter the

Beach Group ID represents the cell zones sharing the damping length containing the same input parameters.

Multi-Directional Beach helps to suppress the numerical reflections that arise from multiple open-channel

pressure outlet boundaries.This is desirable while modeling oblique waves or when the pressure-outlet

boundaries are closer to the zone of interest. (Only available for 3D problems.)

Uni-Directional Beach: should be used to suppress the numerical reflections from a single open channel

pressure outlet.This is the case when the flow is generally uni-directional.

Damping Type allows you to choose between Two Dimensional and One Dimensional.

– Two Dimensional is the damping treatment in the beach and gravity direction.

– One dimensional is the damping treatment in the beach direction.

Compute From Inlet Boundary is set to none by default. If there are available open channel boundaries

(velocity-inlet, pressure-inlet, and mass-flow-inlet), boundary names are added to the drop-down list. If

you select a boundary from the list, the Level Inputs, Uni-Directional Beach Inputs or Multi-Directional

Beach Inputs in beach direction, and Damping Resistance values will be updated in the interface.You

have the option to overwrite the updated inputs with values that are more applicable to your simulation.

Level Inputs is only available for the Two Dimensional damping type.

– Free Surface Level is the same definition as for open channel flow, see Modeling Open Channel

– Bottom Level is the same definition as for open channel flow, see Modeling Open Channel Flows (p. ).

During the automatic calculation from the velocity inlet boundary for short gravity waves, this parameter

is updated under some assumptions, as noted in Solution Strategies (p. ).The bottom level is used

for calculating the liquid height.

Numerical Beach Inputs

Numerical beach is assumed as a rectangular domain, where its end-plane (outer surface) is an open

channel pressure outlet boundary and start-plane is a plane parallel to a pressure outlet. Beach direction

is assumed as the direction normal to a pressure outlet. Damping length is the normal distance between

the end and start plane.

Uni-Directional Beach Inputs:

X, Y, and Z are the vector components of the beach outward normal (typically normal to the nearest

pressure outlet).

The end point is calculated by taking the dot product of beach direction with any point lying on

the end plane. Similarly, the start point is calculated as the dot product of beach direction with

any point lying on the start-plane.

Note

The automatically calculated value of the end point is assumed based on the domain

extents for all of the cell zones. Enter your own value if required.

Damping Length Specification is only available if Open Channel Wave BC is enabled in the

Multiphase Model dialog box. There are two options you can choose from:

End Point and Wave Lengths (default).

End and Start Points are the limits of the damping zone.

Multi-Directional Beach Inputs

Number of Beach

The default is , the maximum is .

X-Direction

Y-Direction

Z-Direction

End Point

Damping Length

See Figure . : Numerical Beach Sketch (p. ) for a visual representation of the numerical beach.

Figure . : Numerical Beach Sketch

Relative Velocity Resistance Formulation calculates the source term using relative velocities in the nu-

merical beach zone when using moving/deforming meshes or moving reference frames.

Linear Damping Resistance is the resistance per unit time.

Quadratic Damping Resistance is the resistance per unit length.

.... Solution Strategies

Below are some helpful key points when using the Numerical Beach option:

. The Compute from Inlet Boundary drop-down list is a convenient feature as it provides automatic

inputs, which you should check to make sure the values are reasonable. Some of the provided values

are calculated under certain assumptions:

a.

The bottom level, in the case of short gravity waves, is selected in the velocity inlet dialog box

for open channel wave boundary conditions. Since there is no user input for this parameter,

ANSYS Fluent calculates the bottom level as the value of the free surface level less . times the

wave length.The assumption is that the liquid height is . times the wave length.

b. The automatically calculated value of the end point is assumed based on the domain extents

for all of the cell zones.

. For manual inputs of start and end points, you should verify that these points are calculated correctly

in the beach direction.To check for their validity, subtracting the start point from the end point

should give you a positive value.

. For manual inputs of Free Surface Level and Bottom Level, you should verify that these points are

calculated correctly in the direction opposite to gravity.To check for their validity, subtracting the

bottom level from the free surface level should give you a positive value.

. In case you create separate damping zones, but the damping length is not sufficient to suppress

the waves, clubbing of the beach could be done by selecting the same beach ID for other cell zones.

In this case, both the cell zones would share the same information.

. In case of separate damping zones (without clubbing), you should verify that the damping length

is more than or equal to the specified number of wave lengths for the calculation of the start point.

. Damping resistance should be chosen carefully as too much or too little damping could affect the

wave profiles in a no-damping zone.The Compute From Inlet Boundary option automatically

populates the values for damping resistances based on analytical correlations for wave energy.

However, you may need to further tune these values for certain cases if the computed values are

found to be unsuitable.

. Steep damping at the beginning of the damping zone could affect the wave profile just before the

damping zone.

. It is recommended that you use a coarse mesh in the damping zone with increased coarseness to-

wards the end of the damping zone.

Instructions for specifying the necessary information for the primary and secondary phases and their

interaction in a VOF calculation are provided below.

Important

In general, you can specify the primary and secondary phases whichever way you prefer. It

is a good idea, especially in more complicated problems, to consider how your choice will

affect the ease of problem setup. For example, if you are planning to patch an initial volume

fraction of  for one phase in a portion of the domain, it may be more convenient to make

that phase a secondary phase. Also, if one of the phases is a compressible ideal gas, it is

recommended that you specify it as the primary phase to improve solution stability.

.... Defining the Primary Phase

To define the primary phase in a VOF calculation, perform the following steps:

. Select phase- in the Phases list.

. Click Edit... to open the Primary Phase dialog box (Figure . :The Primary Phase Dialog Box (p. )).

Figure . : The Primary Phase Dialog Box

. In the Primary Phase dialog box, enter a Name for the phase.

. Specify which material the phase contains by choosing the appropriate material in the Phase Material

. Define the material properties for the Phase Material.

a.

Click Edit..., and the Edit Material dialog box will open.

b. In the Edit Material dialog box, check the properties, and modify them if necessary. (See Physical

Properties (p. ) for general information about setting material properties, Modeling Compressible

Flows (p. ) for specific information related to compressible VOF calculations, and Modeling Solidi-

fication/Melting (p. ) for specific information related to melting/solidification VOF calculations.)

Important

If you make changes to the properties, remember to click Change before closing

the Edit Material dialog box.

. Click OK in the Primary Phase dialog box.

.... Defining a Secondary Phase

To define a secondary phase in a VOF calculation, perform the following steps:

. Select the phase (for example, phase-) in the Phases list.

. Click Edit... to open the Secondary Phase dialog box (Figure . :The Secondary Phase Dialog Box

for the VOF Model (p. )).

Figure . : The Secondary Phase Dialog Box for the VOF Model

. In the Secondary Phase dialog box, enter a Name for the phase.

. Define the material properties for the Phase Material, following the procedure outlined above for setting

the material properties for the primary phase.

. Click OK in the Secondary Phase dialog box.

.... Including Surface Tension and Adhesion Effects

As discussed in When Surface Tension Effects Are Important in the Theory Guide, the importance of

surface tension effects depends on the value of the capillary number, Ca (defined by Equation .

in the Theory Guide), or the Weber number, We (defined by Equation . in the Theory Guide).

Surface tension effects can be neglected if Ca

or We

.

If you want to include the effects of surface tension along the interface between one or more pairs

of phases, as described in Surface Tension and Adhesion in the Theory Guide, right-click Phase Inter-

actions (under the Setup/Models/Multiphase tree item) and select Edit... to open the Phase Inter-

action Dialog Box (p. ) (Figure . : The Phase Interaction Dialog Box (Surface Tension Tab) (p. )).

Setup → Models → Multiphase → Phase Interactions

Edit...

Edit...

Figure . : The Phase Interaction Dialog Box (Surface Tension Tab)

Perform the following steps to model surface tension (and, if appropriate, include adhesion) effects

along the interface between one or more pairs of phases:

. In the Surface Tension tab, enable the Surface Tension Force Modeling option to include the surface

tension method.

Note

Make sure you specify the Surface Tension Coefficients as constant or user-defined.

If none is selected, then Surface Tension Force Modeling will automatically be disabled.

. Select the surface tension method that is most applicable to your case.You can choose between Con-

tinuum Surface Force and Continuum Surface Stress. Information about each of the methods is de-

scribed in Surface Tension in the Theory Guide.

. For each pair of phases between which you want to include the effects of surface tension, specify an input

for the surface tension coefficients using one of the following options:

Temperature-dependent polynomial, piecewise polynomial, or piecewise linear

Note

These options are available while modeling energy.

User-defined surface tension coefficient

Note

This can be defined as a function of any space variable or time.

See Surface Tension and Adhesion in the Theory Guide for more information on surface tension,

and the Fluent Customization Manual for more information on user-defined functions. All surface

tension coefficients are equal to  by default, representing no surface tension effects along the

interface between the two phases.

Important

Important

For calculations involving surface tension, it is recommended that you also turn on the

Implicit Body Force treatment for the Body Force Formulation in the Multiphase

Model dialog box. This treatment improves solution convergence by accounting for

the partial equilibrium of the pressure gradient and surface tension forces in the mo-

mentum equations. See Including Body Forces (p. ) for details.

. If you want to include wall adhesion, enable the Wall Adhesion option and then specify the contact

angle at each wall as a boundary condition (as described in Steps for Setting Boundary Conditions (p. )).

. If you want to include jump adhesion, enable the Jump Adhesion option.When Jump Adhesion is en-

abled, you will need to specify the contact angle at the porous jump in the Porous Jump dialog box (as

described in Defining Multiphase Cell Zone and Boundary Conditions (p. )).The contact angle specific-

ation and measurement for jump adhesion is similar to that of wall adhesion (as explained in step

above).

Important

Jump adhesion only supports the cell based smoothing option for surface tension.

When the Jump Adhesion option is enabled in the Phase Interaction dialog box, the

correct settings are automatically set for surface tension. To view the surface tension

settings, use the solve/set/surface-tension text command.

Note

The following limitations exist:

When the Wall Adhesion and Jump Adhesion options are enabled, you must specify a nonzero

surface tension coefficient.

Jump Adhesion is not available with the Continuum Surface Stress model.

The Continuum Surface Stress model and the Jump Adhesion option are not available with

the Level Set option.

Several surface tension options are provided through the text user interface (TUI) using the

solve/set/surface-tension command :

solve → set → surface-tension

The surface-tension command prompts you for the following information:

whether you require node-based smoothing

The default value is yes, indicating that node-based smoothing will be used. Note that if you are

reading in a case that was created in versions prior to ANSYS Fluent , then cell-based smoothing

will be used by default.

the number of smoothings

The default value is . A higher value can be used in case of tetrahedral and triangular meshes in

order to reduce any spurious velocities.

the smoothing relaxation factor

The default is . This is useful in the cases where volume fraction smoothing causes a problem (for

example, liquid enters through the inlet with wall adhesion on).

whether you want to use volume fraction gradients at the nodes for curvature calculations

With this option, ANSYS Fluent uses volume fraction gradients directly from the nodes to calculate

the curvature for surface tension forces. The default is yes which produces better results with

surface tension compared to gradients that are calculated at the cell centers.

Important

Note that the calculation of surface tension effects will be more accurate if you use a quadrilat-

eral or hexahedral mesh in the area(s) of the computational domain where surface tension is

significant. If you cannot use a quadrilateral or hexahedral mesh for the entire domain, then

you should use a hybrid mesh, with quadrilaterals or hexahedra in the affected areas.

ANSYS Fluent uses node based smoothing for smoothed volume fraction and node based

gradients for smoothed curvature calculation to provide better accuracy and robustness.

Pressure jump caused by the surface tension is discontinuous in nature, and also it acts locally

at the interface.These numerical difficulties are overcome in an approximate manner by con-

sidering the smoothed distribution of the volume fraction field within the finite interfacial

width. Smoothing procedures, in general, are mesh dependent.Therefore, the amount and

nature of the smoothing procedure could have a significant effect on the results for surface

tension cases.

.... Discretizing Using the Phase Localized Compressive Scheme

Most of the interface capturing or tracking schemes, which are common in literature, can simulate

either diffused interface modeling or sharp interface modeling. There are a number of applications

where you may be interested in modeling diffused and sharp interfaces in different regimes, which

results in the need for a unique discretization procedure to handle such applications.

Below are some examples of such applications:

Air bubble rise in water-solid slurry: Diffused interface modeling is required for the water and

solid, and sharp interface modeling for the air bubble is desirable. A sharpening scheme would cause

undesirable effects for the modeling of the diffused interface between water and solids and a diffusive

scheme would not be able to maintain the sharp interface for bubble rising in the slurry.

Evaporation/condensation in a tank partially filled with water and being heated at the bottom:

Diffused interface modeling is required for the liquid-vapor and sharp interface modeling for the

water-air regime is desirable. A sharpening scheme, would not be able to simulate the diffused phe-

nomena of evaporation/condensation for the liquid- vapor phase and a diffusive scheme would not

be able to maintain the sharp interface between water and air.

Air jet penetrating through layer of liquids: You may be interested in diffused jet modeling and

sharp interface modeling between the liquid layers. A sharpening scheme would not be able to

maintain the continuous air stream and a diffusive scheme would not be able to maintain the sharp

interfaces between the layers of liquids.

Using the Modified HRIC and Compressive schemes for such applications would result in the HRIC

scheme producing undesirable sharpening of the dispersed phases and undesirable diffusion of the

continuous phases, whereas the Compressive scheme would produce undesirable sharpening of the

dispersed phases.

Therefore, the phase localized compressive scheme is particularly useful in cases where the desirable

behavior is such that you have diffused modeling of dispersed phases and sharp modeling of continu-

ous phases. In ANSYS Fluent, diffusive and anti-diffusive discretization procedures can be used across

the distinct interfaces, which share a pair of phases. This functionality is provided through the com-

pressive discretization scheme, where the degree of diffusion or sharpness is controlled through the

value of the slope limiters. The theory used is described in The Compressive Scheme and Interface-

Model-based Variants.

Figure . : The Phase Interaction Dialog Box for the VOF Model (Discretization Tab)

To use the phase localized compressive scheme, perform the following steps:

. Click the Discretization tab.

Note

The Discretization tab is available for the VOF model, Mixture multiphase model, and

Eulerian multiphase model with Mulit-Fluid VOF only when the Phase Localized

Discretization option is enabled in the Interface Modeling Options dialog box. (Inter-

face Modeling Type (p. )).

. Enable Phase Localized Compressive Scheme.

Important

When this option is enabled, the Compressive spatial discretization scheme is automat-

ically selected for the Volume Fraction in the Solution Methods dialog box.

. For each pair of phases, specify the value of the slope limiter.You can enter a value of , , or , or any

value between  and . Refer to Table . : Slope Limiter Discretization Scheme (p. ) to equate each

value of the slope limiter with a discretization scheme.

Table . : Slope Limiter Discretization Scheme

Scheme

Slope Limiter Value

first order upwind

second order reconstruction bounded by the global minimum/maximum

of the volume fraction

compressive

Scheme

blended: where a value between  and  means blending of the first order

and second order and a value between  and  means blending of the

second order and compressive scheme

and

When using the Phase Localized Compressive Scheme, note the following:

The minimum limit for the slope limiter is , whereas the maximum is .

The slope limiter can be interpreted as the degree of compression/anti-diffusion, where  demonstrates

the minimum compression and  demonstrates the maximum compression.

For interfaces sharing the diffused phases, a slope limiter value of  should not be used. A value

between  and  is recommended.

For interfaces sharing the continuous phases, any value between  and  can be used depending on

the application.

For interfaces sharing the continuous and diffused phases, any value between  and  can be used

based on the application.

If you want variable discretization behavior for an interface between two phases, you can do so via

the DEFINE_PROPERTY user-defined function.

Note

– If the interface has a transition from sharp to diffused modeling, you should not exper-

ience any problems.

– If the interface has a transition from diffused to sharp modeling, this transition should

be smooth by gradually varying the value of the slope limiter within some transition

zone.

... Setting Time-Dependent Parameters for the Explicit Volume Fraction

Formulation

If you are using the Explicit volume fraction formulation in ANSYS Fluent, an explicit solution for the

zone.

volume fraction is obtained either once each time step or once each iteration, depending upon your

inputs to the model. You also have control over the time step used for the volume fraction calculation.

You can access the controls for the volume fraction from the Multiphase Model Dialog Box (p. ) by

clicking Expert Options...

There are two inputs for the time-dependent calculation for the VOF model:

When ANSYS Fluent uses the Explicit formulation, the time step used for the volume fraction calculation

will not be the same as the time step used for the rest of the transport equations. ANSYS Fluent will refine

the time step for VOF automatically, based on your input for the maximum Courant Number allowed

near the free surface.The Courant number is a dimensionless number that compares the time step in a

calculation to the characteristic time of transit of a fluid element across a control volume.

The characteristic transit time for a fluid element across the control volume represents the time

taken by the fluid to empty out of the cell. This transit time is taken as the smallest of such time

in the region near the fluid interface. A sub time step, for use in the VOF calculations, is computed

based on this characteristic time, and the maximum allowed Courant Number set in the Multiphase

Model Dialog Box (p. ). For example, if the maximum allowable Courant Number is . (de-

fault), the computed sub time step will have a maximum value equal to a quarter of the minimum

transit time for any cell near the interface.

In Fluent, the sub time step size for VOF calculations can be computed using the following options:

Velocity Based: The sub time step is estimated by the cell size and the fluid velocity normal to

the interface:

(.)

where,

is the Courant Number,

is the fluid velocity, and

is the cell size.

Flux Based: For this option, the sub time step is estimated based on the cell volume and the

summation of outgoing fluxes in the cell:

(.)

where,

is the volume, and

are the outgoing fluxes.

Flux Averaged: The sub time step size is estimated by volumetric averaging the calculations of

the Flux Based method for the neighboring cells.

Hybrid: This is the default method for calculating sub time step size. The sub time step size is

estimated by blending the Velocity Based and Flux Averaged calculation methods.

Note

The Flux Based calculation method is the most conservative sub-time step size

estimation, while the Velocity Based calculation is the most aggressive. Flux Aver-

aged and Hybrid methods fall in between for most cases.

Aggressive sub time step calculation methods generally save time during interface

reconstruction. However, the aggressive method can lead to increased number of

iterations due to larger transient errors being introduced while integrating over

the sub time steps for the interface reconstruction.

By default, ANSYS Fluent will solve the volume fraction equation(s) once for each time step.This means

that the convective flux coefficients appearing in the other transport equations will not be completely

updated each iteration, since the volume fraction fields will not change from iteration to iteration.

When ANSYS Fluent solves these equations every iteration, the convective flux coefficients in the

other transport equations will be updated based on the updated volume fractions at each iteration.

This choice is the less stable of the two, and requires more computational effort per time step than

the default choice.

Important

If you are using sliding meshes, or dynamic meshes with layering and/or remeshing,

using the Solve VOF Every Iteration option will yield more accurate results, although

at a greater computational cost.

If you are including melting or solidification in your VOF calculation, note the following:

It is possible to model melting or solidification in a single phase or in multiple phases.

For phases that are not melting or solidifying, you must set the latent heat ( ), liquidus temperature (

),

and solidus temperature (

) to zero.

See Modeling Solidification and Melting (p. ) for more information about melting and solidification.

... Using the VOF-to-DPM Model Transition for Dispersion of Liquid in

Gas

For the analysis of dispersion of liquid in gas, two principal multiphase flow methodologies can be

applied:

In the Euler-Lagrange approach, discrete droplets are tracked through the domain.The particle tracker

uses physical properties of individual droplets in order to account for the exchange of mass, momentum,

heat, species (and so on) with the continuous phase.The gas volume displacement by the droplets is ignored.

This approach is relatively computationally inexpensive because it allows the mesh to be coarser than the

size of a droplet.The secondary breakup can be modeled relatively accurately using known breakup

models. However, in the dense region of a spray, simulation accuracy may suffer from neglecting the volume

displacement. Also, in regions where the spray does not consist of discrete spherical droplets, special

models must be used to predict the primary breakup of the initial contiguous liquid jet.These models must

be derived from experimental data based upon the operating conditions for each injector.

In the volume-of-fluid (VOF) approach, the volume fraction of the liquid is stored in each cell.The gas-liquid

interface can be tracked by explicit discretization schemes, such as geometric reconstruction.The VOF

model requires a much higher mesh resolution and much smaller time steps.The phase boundary around

every droplet must be resolved by a mesh that is significantly finer than the finest droplets.This allows for

better predictions of the primary breakup.The volume displacement is inherently accounted for, which

can be important for the dense region of the dispersed spray. However, this method is expensive and requires

large HPC resources.

ANSYS Fluent provides the capability to combine the two approaches described above by using a VOF-

to-DPM model transition mechanism. The initial jet and primary breakup are predicted using the VOF

model on a sufficiently fine mesh, while the voluminous dilute region of the dispersed spray is simulated

by the DPM. The VOF-to-DPM model transition algorithm automatically finds compact liquid masses

that have detached from the liquid core in the VOF solution. It then assesses their eligibility for the

VOF-to-DPM model transition. If the liquid lump satisfies user-specified criteria, such as lump size and

asphericity (that is, relative or normalized deviation from the shape of a perfect sphere), it is removed

from the resolved liquid in the VOF simulation and converted to a particle parcel in the Lagrangian

formulation. Any local solution-adaptive (such as hanging-node) mesh refinement used to resolve the

gas-liquid interface is automatically reverted, so that the Lagrangian particle parcel can be placed in

a single large cell. If the volume of a liquid lump is much larger than the volume of the coarsened

mesh cell, then the lump will be converted into as many Lagrangian particle parcels as the number of

cells spanned by the lump such that the volume of each parcel will be equal to its corresponding cell

volume. In early stages after the conversion, the group of particle parcels representing the liquid

droplet will travel together, but as they proceed through the domain, their paths may gradually diverge.

Converting liquid lumps to Lagrangian parcels does not impose volume displacement on the continuous-

phase VOF flow simulation. In order to avoid spurious momentum sources, a volume of gas with the

same volume as the liquid lump is created in the VOF simulation to maintain the volume conservation.

The mass source that is equivalent to the mass of the gas volume will affect the overall mass balance.

This approach can be used for simulating liquid atomization in gas turbines, internal combustion engines,

and other similar applications.

Such simulations usually require high spatial and temporal resolution to capture all the relevant details

of a primary atomization process of a liquid jet. Resource limitations will restrict this approach to detailed

analyses in regions near the nozzle. For the complete simulation of a spray system or process, it is re-

commended that all information about the Lagrangian DPM particle parcels be captured and transferred

into a separate simulation that only uses the Euler/Lagrange approach because it allows a coarser

mesh and larger time steps to be used.

This can be achieved, for example, by using DPM particle sampling on either a cut plane or the outlet

boundary of the domain of the detailed VOF-to-DPM simulation. For unsteady particle tracking, the

sampling feature writes information into a file for every particle parcel that crosses the sampling plane

or boundary. The file can then be used as an unsteady injection file for another unsteady particle

tracking simulation. ANSYS Fluent will recreate each particle parcel at the same location and instance

in simulated time (flow-time in the injection file).

An alternative to using DPM particle sampling for creating such a file is to use the VOF-to-DPM built-

in functionality as described below. If you provide a filename, the solver will write a new file containing

information for each liquid lump that has been converted. The file has the same format as a DPM

sample file for unsteady particle tracking. Therefore, it can be read into a separate DPM simulation as

an unsteady injection file.

.... Limitations on Using the VOF-to-DPM Model Transition

The VOF-to-DPM model transition feature cannot be used with the following:

– Steady-state flow

– Multi-fluid VOF

– Steady DPM particle tracking

– The Level Set model

The identification of individual lumps and the calculation of the lump properties do not account for special

boundary conditions such as symmetry and periodicity (including periodic non-conformal interfaces). A

liquid lump that touches a symmetry boundary is treated as if it was attached to a wall. A lump that inter-

sects a periodic boundary is treated as multiple independent lumps. In both cases, the values calculated

for the lump properties, particularly the asphericity, will be affected.

Important

The VOF-to-DPM model transition mechanism is available only for 3D cases.

.... Setting up the VOF-to-DPM Model Transition

To use the VOF-to-DPM Model Transition capability, follow the steps below:

. When generating the mesh for your analysis, avoid high-aspect-ratio cells. Adjust the mesh resolution

so that four or five levels of hanging-node refinement will be sufficient for resolving the finest structures

when you are using the VOF calculation.

. If appropriate, define the dynamic solution-adaptive (hanging-node) mesh refinement.

Domain → Adapt → Refine/Coarsen...

For example, if you just want to make sure that the phase boundary is resolved with the highest

possible mesh resolution, you can use cell registers that apply the Curvature method to the phase

volume fraction in order to coarsen all cells with a value below .e- and refine all cells with a

value above .e-. Make sure to select Dynamic Adaption and use a small Frequency (such as

or ).

If the resolution of the initial mesh is not uniform, you can specify a minimum cell volume in the

Adaption Controls dialog box in order to avoid excessively small cells (and therefore high CFL

numbers), or when multiphase-specific time stepping is used, to avoid excessively small time-

steps. If a sufficient number of refinement levels is specified, the adapted mesh at the liquid/gas

interface will have little variation in cell volume, regardless of the local resolution in the initial

mesh.

If you use hanging nodes to create the initial mesh, make sure that you use the polyhedral un-

structured mesh adaption (PUMA) for the dynamic solution-adaptive mesh refinement, because

the conventional mesh adaption will skip two cell layers on the coarse side of the hanging nodes.

To activate PUMA, use the following text command:

mesh/adapt/set/method

. In the Discrete Phase Model dialog box, select Unsteady Particle Tracking.

Physics → Models → Discrete Phase...

. Create a DPM injection of any type as usual and specify a very large value for Start Time.This will guar-

antee that no particles will be injected at the specified location.

New...

. In the Multiphase Model dialog box, configure the following settings.

Physics → Models → Multiphase...

Value

Setting

Tab

(Selected)

Volume of Fluid

Model

Explicit

Volume Fraction

Sharp

Type

Interface Modeling

Implicit Body Force

Body Force Formulation

. In the Phase Interaction dialog box in the Surface Tension tab, define the correct surface tension for

the gas-liquid boundary.

Edit...

. In the Solution Methods task page, configure the following solution parameters.

Solution → Solution → Methods...

Value

Setting

Group Box

PISO

Scheme

Pressure-Velocity Coupling

Spatial Discretization

PRESTO! or Body Force

Weighted

Pressure

. If you selected PISO for the Pressure-Velocity Coupling scheme, increase the Pressure and Momentum

Under-Relaxation Factors to values close to  (for example, .) in the Solution Controls task page.

Solution → Controls → Controls...

. In the Phase Interaction dialog box, in the Mod.Trans'on tab, define VOF-to-DPM model transition.

Edit...

a.

Specify the Number of Model Transition Mechanisms.

b. For each mechanism, select the liquid phase from the Phase to be Converted drop-down list and

also the gas phase from the Volume-balancing Eulerian Phase drop-down lists.

Lagrangian particle parcels do not have any volume displacement effect on any VOF phase.

Therefore, in order to maintain volume conservation in the VOF solution, when liquid from

the VOF solution is converted into one or more Lagrangian particle parcel(s), an equal volume

of the selected gas phase is placed into the VOF solution as a replacement for the converted

liquid.

c.

For each pair of phases with model transition, select vof-to-dpm from the Mechanism drop-down

list.

Figure . : The VOF-to-DPM Parameters Dialog Box

d. In the VOF-to-DPM Parameters dialog box that opens automatically, specify the parameters for the

model transition:

Frequency (do every N time steps)

specifies the frequency at which the VOF-to-DPM model transition mechanism is run.

Injection

is a list of available injections. Make sure you select the injection that you created earlier for the

VOD-to-DPM model transition. All newly created particle parcels will be assigned to the selected

injection.

Coarsen the Mesh when Lumps are Converted

specifies whether the mesh should be coarsened when a liquid lump is converted to a DPM

particle parcel and removed from the VOF solution.The coarsening is achieved by reverting all

previously dynamically added mesh refinements.This option is selected by default and recom-

mended.

Split any DPM Parcel that Exceeds the Cell Volume by Factor

specifies a ratio used for determining the number of DPM parcels into which the liquid lump is

mended.

divided. If the liquid lump volume does not exceed the volume of the coarsened cell multiplied

by this factor, the lump is converted into one parcel containing one particle. Otherwise, the lump

is split into as many parcels as there are cells covered by the original liquid lump.To conserve

mass, the number of particles per parcel is reduced from unity such that the sum of all parcels

resulting from the split represents exactly the mass of the original liquid lump.

The splitting of a single lump into multiple particle parcels may be needed if there is a risk

that DPM source terms may cause instabilities in the continuous phase flow solution. This

may happen for cases with evaporation or boiling and a fine background mesh.

As long as you do not encounter any stability issues in the continuous phase flow solution,

you can set a very high value for this factor in order to prevent lumps from splitting into

multiple parcels. However, if the factor is set relatively low, a lump may split into multiple

parcels. These parcels are mutually independent and therefore may disperse. Splitting

parcels does not change the global size distribution, but they may affect the spatial distri-

bution of parcels of different sizes throughout the spray.

VOF Lumps Conversion Requirements

contains parameters for specifying conversion eligibility limits.

Volume-Equivalent Sphere Diameter Range

sets the Minimum and Maximum diameter values for a volume-equivalent sphere. Liquid

droplets found in the VOF solution whose volume is outside this range will not be converted

to Lagrangian particle parcels.

Upper Limits of Asphericity as Calculated by

Maximum Asphericity by Radius Std. Dev.

specifies the maximum asphericity calculated from the normalized radius standard devi-

ation.This quantity is calculated for every liquid lump found in the VOF solution as follows.

For every facet of the lump surface (gas-liquid phase interface), the distance between the

facet center and the lump center of gravity is calculated.The individual distance values

are weighted by the size of the individual lump boundary facet.Their standard deviation

is computed and then normalized by the average radius.

This quantity is zero for perfect spheres and increasingly greater than zero the

more the shape deviates from a sphere. All droplets for which the asphericity value

is below the specified maximum may be automatically elected for conversion. The

default value for Maximum Asphericity by Radius Std. Dev. is ..

Maximum Asphericity by Radius-Surface Orthogonality

specifies the maximum asphericity calculated from the average radius-surface orthogon-

ality.This quantity is calculated for every liquid lump found in the VOF solution as follows.

For every facet of the lump surface (gas-liquid phase interface), a vector from the lump's

center of gravity to the center of the lump boundary facet is computed.This vector is

normalized and then used in a dot product with the facet unit normal to yield a measure

of a relative orthogonality ranging from  to . For a perfect sphere, the value would all

be . A facet area-weighted average of these values is then subtracted from  to obtain

the asphericity value.

For almost spherical droplets, this quantity is significantly closer to  than the

standard deviation-based asphericity. For more drastically non-spherical lumps, it

produces values comparable to those obtained with the standard deviation-based

asphericity. The default value for Maximum Asphericity by Radius-Surface Ortho-

gonality is ..

Lump Conversion Transcript File Name (empty for none)

(optional) specifies a name for the file where ANSYS Fluent will save the DPM particle variables

corresponding to each VOF lump that is converted.The file contains one line for each converted

lump, regardless of whether a lump was converted into one or multiple DPM parcels.The file is

written in the same format that is used for particle sampling (see Sampling of Trajectories (p. )).

As with any sample file written by unsteady particle tracking, this file can be used as an

unsteady injection file. This makes it possible to calculate the small dense region of a spray

using the VOF-to-DPM model transition mechanism and the much larger dilute region in

a pure DPM calculation that uses the lump conversion transcript as an injection file. For

better control over the number of the numerical particle parcels, the injection file can be

run through the file reduction tool as described in Data Reduction of Samples (p. ).

If you use a DEFINE_DPM_OUTPUT UDF to write the particle sampling file, the same UDF

will be used to write the lump conversion transcript file. The UDF gives you control over

the file content and it even allows you to modify the DPM particle parcels generated from

the liquid lumps during the VOF-to-DPM model transition. For details, see

DEFINE_DPM_OUTPUT in the Fluent Customization Manual.

You can use the DEFINE_DPM_OUTPUT UDF to add additional DPM variables to the

output file in extra columns. If you then use that lump conversion transcript file as an un-

steady injection file in a separate simulation, you can use a DEFINE_DPM_INJEC-

TION_INIT UDF to read the additional columns and use the data to initialize the addi-

tional DPM variables. For details, see DEFINE_DPM_INJECTION_INIT in the Fluent

Use this Mechanism for Lump Postprocessing

when selected, ANSYS Fluent uses the mechanism settings for the calculation of the postprocessing

lump detection quantities. See Postprocessing for VOF-to-DPM Model Transition Calcula-

tions (p. ) for information about postprocessing lump detection quantities.

The liquid lumps having dimensions within the specified lump diameter range and falling below

both the asphericity criteria will be elected for conversion to DPM parcels.

In order to see typical asphericity values for the droplets in your simulation, you can, for ex-

ample, create contour plots of the asphericity field functions on an iso-surface of a volume

fraction of ..

.... Postprocessing for VOF-to-DPM Model Transition Calculations

The following additional postprocessing variables will become available for postprocessing under the

Lump Detection... category:

Lump ID

Lump Diameter

Lump Density

Lump Asph. by Rad. Std. Dev.

Lump Asph. by Orthogonality

Lump X,Y, Z Coordinate

Lump X,Y, Z Velocity

Lump Temperature

When the energy equation is enabled, the following additional variables are available for postprocessing

under the Lump Detection... category:

Lump Enthalpy

Lump Pressure

.. Setting Up the Mixture Model

For background information about the mixture model and the limitations that apply, refer to Overview

... Defining the Phases for the Mixture Model

... Including Mixture Drift Force

... Including Cavitation Effects

... Including Semi-Mechanistic Boiling

interaction for a mixture model calculation are provided below.

The procedure for defining the primary phase in a mixture model calculation is the same as for a VOF

calculation. See Defining the Primary Phase (p. ) for details.

.... Defining a Non-Granular Secondary Phase

To define a non-granular (that is, liquid or vapor) secondary phase in a mixture multiphase calculation,

perform the following steps:

. Click Edit... to open the Secondary Phase Dialog Box (p. ) (Figure . :The Secondary Phase Dialog

Box for the Mixture Model (p. )).

Setting Up the Mixture Model

Figure . : The Secondary Phase Dialog Box for the Mixture Model

. Define the material properties for the Phase Material, following the same procedure you used to set

the material properties for the primary phase (see Defining the Primary Phase (p. )). For a particulate

phase (which must be placed in the fluid materials category, as mentioned in Steps for Using a Multiphase

Model (p. )), you need to specify only the density; you can ignore the values for the other properties,

since they will not be used.

. In the Properties group box, specify the Diameter of the bubbles, droplets, or particles of this phase

(

in Equation . in the Theory Guide).You can specify a constant value, or use a user-defined

function. See the Fluent Customization Manual for details about user-defined functions. Note that when

you are using the mixture model without slip velocity, this input is a characteristic length scale.

.... Defining a Granular Secondary Phase

To define a granular (that is, particulate) secondary phase in a mixture model multiphase calculation,

Box for a Granular Phase Using the Mixture Model (p. )).

Figure . : The Secondary Phase Dialog Box for a Granular Phase Using the Mixture Model

the material properties for the primary phase (see Defining the Primary Phase (p. )). For a granular

Important

Note that all properties for granular flows can be defined by user-defined functions

(UDFs).

. Enable the Granular option.

. In the Properties group box, specify the following properties of the particles of this phase:

Diameter

specifies the diameter of the particles.You can select constant in the drop-down list and specify a

constant value, or select user-defined to use a user-defined function. See the Fluent Customization

Granular Viscosity

specifies the method for computing the kinetic (

) and collisional (

) components of the

granular viscosity (Equation . in the Fluent Theory Guide). Selecting constant, syamlal-obrien

(Equation . in the Fluent Theory Guide), or gidaspow (Equation . in the Fluent Theory Guide)

will use these expressions for the kinetic portion of the viscosity and will calculate the collisional

portion of the viscosity from Equation . in the Fluent Theory Guide. Alternatively, you can select

user-defined to use a user-defined function. Note that if you select user-defined, your user-defined

function must include both the kinetic portion and the collisional portion of the viscosity in the value

it returns.

Frictional Pressure

specifies the pressure gradient term,

, in the granular-phase momentum equation. Choose

none to exclude frictional pressure from your calculation, johnson-et-al to apply Equation .

in the Theory Guide, syamlal-obrien to apply Equation . in the Theory Guide, based-ktgf,

where the frictional pressure is defined by the kinetic theory  [] (p. ).The solids pressure tends

to a large value near the packing limit, depending on the model selected for the radial distribution

function.You must hook a user-defined function when selecting the user-defined option. See the

Fluent Customization Manual for information on hooking a UDF.

Frictional Modulus

(.)

with

, which is the derived option. You can also specify a user-defined function for the

frictional modulus.

Friction Packing Limit

specifies a threshold volume fraction at which the frictional regime becomes dominant.The default

value is ..

specifies temperature for the solids phase and is proportional to the kinetic energy of the random

value is ..

motion of the particles. Choose either the algebraic, the constant, or user-defined option.

Solids Pressure

, in the granular-phase momentum equation. Choose either

the lun-et-al, the syamlal-obrien, the ma-ahmadi, or the user-defined option.

Radial Distribution

specifies a correction factor that modifies the probability of collisions between grains when the solid

granular phase becomes dense. Choose either the lun-et-al, the syamlal-obrien, the ma-ahmadi,

the arastoopour, or a user-defined option.

Elasticity Modulus

(.)

with

.

Choose either the derived or user-defined options.

Packing Limit

specifies the maximum volume fraction for the granular phase. For monodispersed spheres, the

packing limit is about ., which is the default value in ANSYS Fluent. In polydispersed cases, however,

smaller spheres can fill the small gaps between larger spheres, so you may need to increase the

maximum packing limit.

.... Defining the Interfacial Area Concentration via the Transport Equation

If you want to solve the transport equation for interfacial area concentration of the secondary phase

in the mixture model (Interfacial Area Concentration in the Fluent Theory Guide, perform the following

steps:

Box Displaying the Interfacial Area Concentration Settings (p. )).

Figure . : The Secondary Phase Dialog Box Displaying the Interfacial Area Concentration

Settings

. Enable the Interfacial Area Concentration option. Make sure the Granular option is disabled for the

Interfacial Area Concentration option to be visible in the interface.

Diameter

specifies the diameter of the particles or bubbles.You can select constant in the drop-down list and

specify a constant value, or select user-defined to use a user-defined function. See the Fluent Cus-

tomization Manual for details about user-defined functions.The Diameter recommended setting is

sauter-mean, allowing for the effects of the interfacial area concentration values to be considered

for mass, momentum and heat transfer across the interface between phases.

Surface Tension

specifies the surface tension at the liquid-air interface.You can select either the hibiki-ishii or the

ishii-kim model.

Coalescence Kernel and Breakage Kernel

allows you to specify the coalescence and breakage kernels.You can select none, constant, hibiki-

ishii, ishii-kim, yao-morel, or user-defined.The three options, hibiki-ishii, ishii-kim and yao-morel

are described in detail in Interfacial Area Concentration in the Theory Guide.

In addition to specifying the hibiki-ishii, ishii-kim, and yao-morel as the coalescence and

breakage kernels, you can also tune the properties of the three models by using the

/define/phases/iac-expert/hibiki-ishii-model, /define/phases/iac-

expert/ishii-kim-model, and /define/phases/iac-expert/yao-morel-model

text commands.

For each of the three models you can specify the parameters listed in Table . : Parameters

for the Coalescence and Breakage Kernels (p. )

Table . : Parameters for the Coalescence and Breakage Kernels

Yao-Morel Model

Ishii-Kim Model

Hibiki-Ishii

Coefficient K_c1

Coefficient Crc

Coefficient Gamma_c

Coefficient K_c3

Coefficient Cwe

Coefficient K_c

Coefficient K_b1

Coefficient C

Coefficient Gamma_b

alpha_max

Coefficient Cti

Coefficient K_b

alpha_max

alpha_max

These values are discussed in greater detail in Interfacial Area Concentration in the Theory

Guide.

Nucleation Rate

is a source term for the interfacial area concentration that models the rate of formation of the dispersed

phase.You can choose from constant or user-defined.

Critical Weber Number

will need to be specified if you selected ishii-kim or yao-morel for the Breakage Kernel.

Dissipation Function

gives you the option to choose the formula which calculates the dissipation rate used in the hibiki-

ishii and ishii-kim models.You can choose amongst constant, wu-ishii-kim, fluent-ke, and user-

defined for the dissipation function.

The wu-ishii-kim option uses a simple algebraic correlation for :

(.)

where

and

where

,

,

, and

(.)

where

and

where

,

,

, and

are the mixture density, mixture velocity, mixture molecular viscosity,

and hydraulic diameter of the flow path.

When you select the wu-ishii-kim model, you will set an additional input for Hydraulic Dia-

meter.

Hydraulic Diameter

is the value used in Equation . (p. ), should you use the wu-ishii-kim formulation.

Min/Max Diameter

are the limits of the bubble diameters.

Note

When solving a steady-state problem, the preferred setting for the Under-Relaxation

Factor is ., as the interfacial area equation for the boiling models is currently under-re-

laxed using a locally defined pseudo-time step. If you want extra explicit under-relaxation,

you may set the value of the Under-Relaxation Factor to less than one, this may be done

only in case of serious convergence problems with the interfacial area transport equation.

To improve convergence you can switch to a pseudo-time step for the interfacial area

concentration only, using the define/phases/iac-expert/iac-pseudo-time-step text com-

mand and set the local pseudo-time to less than .

.... Defining the Algebraic Interfacial Area Concentration

If you have chosen not to solve the transport equation for Interfacial Area Concentration (Defining

the Interfacial Area Concentration via the Transport Equation (p. )), then you can select an algeb-

raic model to estimate the interfacial area from the secondary phase diameter specified in the Sec-

ondary Phase Dialog Box (p. ). To choose an algebraic interfacial area model perform these steps.

. In the tree, right-click Phase Interactions (under Setup/Models/Multiphase) and select Edit... to open

the Phase Interaction dialog box.

. In the Interfacial Area tab, select the desired algebraic model for the Interfacial Area. Note the following

regarding the available choices:

ia-symmetric

considers both the primary and secondary phase volume fractions in estimating the interfacial area.

ia-gradient

considers the volume fraction gradient at the interface between two phases in estimating the inter-

facial area.

See DEFINE_EXCHANGE_PROPERTY in the Fluent Customization Manual.

In addition to these models, ANSYS Fluent provides the Gradient-Symmetric model, which is available

via the text user interface. You can use the following text commands to enable this model:

solve/set/multiphase-numerics/heat-mass-transfer/area-density/ia-grad-

sym?

switch to ia-grad-symmetric option? [yes] yes

See Algebraic Models in the Fluent Theory Guide for details about the theory behind algebraic interfacial

area models.

.... Defining Drag Between Phases

For mixture multiphase flows with slip velocity, you can specify the drag function to be used in the

calculation. The functions available here are a subset of those discussed in Defining the Phases for

the Eulerian Model (p. ). See Relative (Slip) Velocity and the Drift Velocity in the Theory Guide for

more information.

To specify drag laws, click Interaction... to open the Phase Interaction Dialog Box (p. ) (Fig-

ure . : The Phase Interaction Dialog Box for the Mixture Model (Drag Tab) (p. )), and then click

the Drag tab.

Figure . : The Phase Interaction Dialog Box for the Mixture Model (Drag Tab)

.... Defining the Slip Velocity

If you are solving for slip velocities during the mixture calculation, and you want to modify the slip

velocity definition, click Interaction... to open the Phase Interaction Dialog Box (p. ) (Fig-

ure . : The Phase Interaction Dialog Box for the Mixture Model (Slip Tab) (p. )), and then click

the Slip tab.

Figure . : The Phase Interaction Dialog Box for the Mixture Model (Slip Tab)

Under Slip Velocity, you can specify the slip velocity function for each secondary phase with respect

to the primary phase by choosing the appropriate item in the adjacent drop-down list.

Select maninnen-et-al (the default) to use the algebraic slip method of Manninen et al. [] (p. ), de-

scribed in Relative (Slip) Velocity and the Drift Velocity in the Theory Guide.

Select none if the secondary phase has the same velocity as the primary phase (that is, no slip velocity).

Select user-defined to use a user-defined function for the slip velocity. See the Fluent Customization

Manual for details.

.... Including Surface Tension and Wall Adhesion Effects

You can include the effects of surface tension along the interface between one or more pairs of phases

as described in Including Surface Tension and Adhesion Effects (p. ). For more information about

the theoretical background, see Surface Tension and Adhesion in the Fluent Theory Guide.

Note

Note

The surface tension option in recommended for cases with sharp/dispersed interface modeling

type.

Jump adhesion is not supported with the Mixture Multiphase model.

If you are solving for slip velocity and using one of the turbulence models in your Mixture multiphase

calculation, you can also include the effects of the slip velocity on the momentum and turbulence

equations. To include these effects, enable Mixture Drift Force in the Viscous Model Dialog Box (p. ).

The turbulent dispersion effect will be included in the slip velocity equation (Equation . in the

Fluent Theory Guide). Note that the inclusion of these terms can slow down convergence noticeably.

If you are looking for additional accuracy, you may want to compute a solution first without these

sources, and then continue the calculation with these terms included. In most cases these terms can

be neglected.

For mixture model calculations, it is possible to include the effects of cavitation, using ANSYS Fluent’s

cavitation models described in Cavitation Models in the Theory Guide.

To enable the Singhal et al. cavitation model, use the solve/set/expert text command and answer

yes to use Singhal-et-al cavitation model?. The Singhal-Et-Al Cavitation Model option

will now be visible in the Phase Interaction dialog box, under the Mass tab. Enable this option to

include the Singhal et al. cavitation model.

You will specify three parameters to be used in the calculation of mass transfer due to cavitation. Set

the Vaporization Pressure, the Surface Tension Coefficient, and the Non-Condensable Gas Mass

Fraction. The default value of

is  Pa, the vaporization pressure for water at ambient temper-

ature. Note that

and the surface tension are properties of the liquid, depending mainly on temper-

ature. Non-Condensable Gas Mass Fraction is the mass fraction of dissolved gases, which depends

on the purity of the liquid.

When multiple species are included in one or more secondary phases, or the heat transfer due to

phase change must be taken into account, the mass transfer mechanism must be defined before enabling

the cavitation model. It may be noted, however, that for cavitation problems, at least two mass transfer

mechanisms are defined:

mass transfer from liquid to vapor.

mass transfer from vapor to liquid.

To enable and set up the Schnerr-Sauer and Zwart-Gerber-Belamri cavitation models, refer to Including

Mass Transfer Effects (p. ).

.... Overview and Limitations for the Semi-Mechanistic Boiling Model

The semi-mechanistic boiling model can be used only with the following models and conditions:

Mixture multiphase

Turbulent kinetic energy-based models (such as -  or -

)

Activated gravity along with zero operating density

Surface tension coefficient (specified in the Phase Interaction dialog box)

Boiling walls with either temperature or conjugate heat transfer boundary conditions

Note

If your case has a boiling wall with heat flux boundary condition, you can add a small

thickness of solid and apply heat flux to the solid boundary. Thus you will be able to

Note

apply heat flux boundary condition indirectly at the boiling wall through conjugate heat

transfer boundary condition.

Binary mixtures with the fixed mixture composition only (pseudo-fluid approach). All the properties and

saturation data for the pseudo-fluid must be provided according to the mixture fixed composition.

For the theoretical background on the semi-mechanistic boiling model, see Semi-Mechanistic Boiling

Model in the Fluent Theory Guide.

.... Using the Semi-Mechanistic Boiling Model

To use the semi-mechanistic boiling model, follow the steps below:

. In the Phase Interaction dialog box, in the Mass tab, specify the Number of Mass Transfer Mechanisms

and then select the liquid and vapor phases in the From Phase and To Phase drop-down lists, respectively.

. Select evaporation-condensation from the Mechanism drop-down list.

. In the Evaporation-Condensation Model dialog box that opens, select Semi-Mechanistic as the Boiling

Model.

The Evaporation-Condensation Model dialog box expands to reveal additional Boiling Paramet-

ers.

Figure . : The Evaporation-Condensation Model Dialog Box

Note

For the Semi-Mechanistic boiling model, the Saturation Temperature can be only

specified using either the tabular-pt-sat or tabular-ptl-sat option.

. In the Boiling Parameters group box, specify the following parameters:

Bulk Temperature

is a temperature of bulk fluid away from the wall.Typically, the inlet temperature of the coolant is

used as the bulk temperature.

is used in the calculation of the reference Reynolds number. It is typically taken to be the hydraulic

diameter.

. To access additional boiling settings for advanced control, select Boiling Model Advanced Settings to

reveal more options.

. In the Boiling Model Reference Quantities group box, you can specify the following:

Reference Velocity

is the velocity of the fluid away from a heated wall at some reference location.This quantity is used

to calculate the reference Reynolds number

in Equation . in the Fluent Theory Guide.You

can choose one of the following specification methods:

ystar-dependent

(default) calculates the reference velocity away from the boiling wall at

=  using standard

wall functions for turbulence. Here,

is a normalized wall distance.You can adjust its value in

the Ystar Far field.

constant

specifies a constant value for the reference velocity.

uses a user-defined function for the reference velocity calculation.

Reference Temperature

is the temperature of fluid away from a heated wall at some reference location (

in the Fluent Theory Guide). Fluid properties used for the reference Reynolds number computation

are calculated at the reference temperature.You can choose one of the following specification

methods:

bulk-temperature

(default) takes the reference temperature from a user-defined Bulk Temperature value.

calculates the reference temperature at

= using standard wall functions for turbulence.

In this case, a value specified for Bulk Temperature serves as the minimum reference temperature.

uses a user-defined function for the reference temperature calculation.

. In the Boiling Methods group box, you can select:

Chen

(default) calculates the boiling heat flux as a weighted superposition of single-phase heat flux (forced

convective) and nucleate boiling heat flux. See Semi-Mechanistic Boiling Model in the Fluent Theory

Guide for details about this method.

uses a framework provided by ANSYS Fluent to hook user-defined correlations for all of the relevant

inputs.

. Enter the value for the Power Law Superposition Constant (  in Equation . in the Fluent Theory

Guide).This constant is used to blend single phase and nucleate boiling heat transfer coefficients based

on asymptotic power law.The default value is .The typical range is from  to .

. In the Single Phase Heat Flux Parameters group, you can set:

Heat Transfer Coefficient: is

in Equation . in the Fluent Theory Guide.The following specific-

ations methods are available:

– standard: Uses a built-in treatment of the heat transfer coefficient for a liquid phase.

– constant

– user-defined

Convective Augmentation Factor: specifies the single-phase heat flux augmentation factor due to

the bubble agitation.The following specification methods are available:

– chen: (default) Uses the correlations proposed by Chen. See Semi-Mechanistic Boiling Model in the

Fluent Theory Guide for more information.

– constant

– constant

This input parameter is available only when Chen is selected in the Boiling Methods group

box.

Heat Flux Multiplier: is an additional factor to adjust a single-phase heat flux (

in the Fluent Theory Guide).This factor can be used when the single phase-heat flux is not predicted

well due to an under-developed turbulent flow, uncertainties in surface roughness, interaction of

thermal and momentum boundary layers when starting from different points or other factors.You

can choose a constant or user-defined specification method.The default value is .

. In the Nucleate Boiling Heat Flux Parameters group, you can set:

Heat Transfer Coefficient:The specification methods are:

– forster-zuber: Uses the nucleate boiling heat transfer coefficient proposed by Forster and Zuber

(Equation . in the Fluent Theory Guide).

– constant

Boiling Suppression Factor: Accounts for the nucleate boiling suppression due to the effect of forced

convection.The presence of bubbles due to local boiling at heated walls augments forced convection

and suppresses nucleate boiling.The following specification methods are available:

– chen-steiner: (default) Uses the modification proposed by Steiner (Equation . in the Fluent

Theory Guide to Equation . in the Fluent Theory Guide). See Semi-Mechanistic Boiling Model in

the Fluent Theory Guide for more information.

– chen: Uses Chen's correlation

(Equation . in the Fluent Theory Guide). See Semi-Mech-

anistic Boiling Model in the Fluent Theory Guide for more information.

– constant

– constant

box.

Heat Flux Multiplier: is an additional factor to adjust a nucleate boiling heat flux (

in Equa-

tion . in the Fluent Theory Guide). Boiling correlations are obtained for a specific pressure and

temperature range for certain materials.This additional heat flux multiplier allows you to tune in heat

transfer coefficient when these correlations are used in generalized sense.You can choose a constant

or user-defined specification method.The default value is .

You can use the DEFINE_MASS_TR_PROPERTY UDF to define input parameters for the semi-

mechansitic boiling model. See DEFINE_MASS_TR_PROPERTY in the Fluent Customization Manual

.... Cell Zone Specific Boiling

By default, boiling is enabled in all the cell zones. When boiling is expected only in certain zones, you

can disable boiling in other zones to make the calculation faster. This can be done by clearing Boiling

Zone in the Fluid dialog box (Multiphase tab).

.... Expert Options for the Semi-Mechanistic Boiling Model

You can access expert options for the semi-mechanistic boiling model by issuing the following text

commands:

solve/set/multiphase-numerics/heat-mass-transfer/boiling/show-expert-

options?

show expert options in semi-mechanistic boiling model? [yes] yes

The evaporation-condensation model dialog box expands to show boiling model expert options.

Figure . : Boiling Model Expert Options

You can adjust the following parameters:

Minimum Superheat

is the minimum superheat required for the onset of nucleate boiling.You can define the Minimum Su-

perheat as:

constant

hsu

The hsu method uses the expression proposed by Hsu [] (p. ):

where

= minimum superheat

= single phase heat transfer coefficient for liquid

The remaining notation is the same as in Semi-Mechanistic Boiling Model in the Fluent Theory

Guide.

Maximum Superheat

is the maximum superheat used in the nucleate boiling heat flux expressions.

Wall Liquid Wetting Fraction

is the area fraction of the wall wetted by liquid. Since a wall may be completely wetted by liquid even

if the neighboring cell liquid volume fraction is below , this is a crucial parameter for the proper estim-

ation of the heat flux.

You can choose one of the following methods:

transition-function

(default) is the wetting fraction that controls the transition from a completely wet to a completely

dry wall state.When the liquid volume fraction in the wall neighboring cells exceeds a value of the

Critical Liquid Volume Fraction that you specified, the wall is assumed to be completely wetted

by liquid.The wetting fraction  is calculated as:

where

= volume fraction of liquid

= Critical Liquid Volume Fraction (default = .)

= transition constant (default = )

The dependency of the wetting function  on the liquid volume fraction

is shown in Fig-

ure . : Transition Function vs. Volume Fraction of Liquid (p. ).

Figure . : Transition Function vs. Volume Fraction of Liquid

wall-neighbor

calculates the wetting fraction through the neighboring cell volume fractions.

constant

constant

allows you to specify the wall liquid wetting fraction as a constant value.

allows you to hook a user-defined function that specifies custom values for the wall liquid wetting

fraction.

.... Solution Strategies for the Semi-Mechanistic Boiling Model

If you face difficulties in convergence for the energy equation while using the conjugate heat transfer

boundary condition, you can use the following strategies:

. Ideally, the semi-mechanistic boiling model is best suited for cases with meshes with y+ > . In the

worst case, y+ should not be less than .

. Use low order schemes for turbulence kinetic energy and momentum.

. Reduce the relaxation factor for turbulence kinetic energy to a value between .-..

. Reduce the relaxation factor for heat flux to a value between .-..

. In case of steady state pseudo-transient simulations that use automatic time-scale, reduce the fluid Time

Scale Factor to ..

. For a large change in heat flux, you can modify the heat flux relaxation factor using the following text

command:

solve/set/multiphase-numerics/heat-mass-transfer/boiling/heat-flux-

relaxation-factor

heat flux relaxation factor for semi-mechanistic boiling model [.]

.

The heat flux relaxation factor will be modified as follows:

where  and

are the new and old heat fluxes, respectively, and

is the heat flux relax-

ation factor that you specified.

Note

To carry out validations against experimental data, you should first run simulations under

Note

non-boiling conditions. If the single-phase heat flux differs from the available data, you

should adjust the single-phase heat flux multiplier prior to carrying out the boiling simula-

tions. There is no unique choice of nucleate boiling correlations; therefore, the default

nucleate boiling correlation is not guaranteed to work under all the operating conditions.

ANSYS Fluent provides flexibility either to tune in the existing methods or to hook user-

defined properties for all supported boiling model inputs.

.. Setting Up the Eulerian Model

For background information about the Eulerian model and the limitations that apply, refer to Overview

of the Eulerian Model in the Theory Guide.

... Additional Guidelines for Eulerian Multiphase Simulations

... Defining the Phases for the Eulerian Model

... Modeling Turbulence

... Including Heat Transfer Effects

... Using an Algebraic Interfacial Area Model

... Including the Dense Discrete Phase Model

... Including the Boiling Model

... Including the Multi-Fluid VOF Model

Once you have determined that the Eulerian multiphase model is appropriate for your problem (as

described in Choosing a General Multiphase Model in the Theory Guide), you should consider the

computational effort required to solve your multiphase problem. The required computational effort

depends strongly on the number of transport equations being solved and the degree of coupling. For

the Eulerian multiphase model, which has a large number of highly coupled transport equations,

computational expense will be high. Before setting up your problem, try to reduce the problem

statement to the simplest form possible.

Instead of trying to solve your multiphase flow in all of its complexity on your first solution attempt,

you can start with simple approximations and work your way up to the final form of the problem

definition. Some suggestions for simplifying a multiphase flow problem are listed below:

Use a hexahedral or quadrilateral mesh (instead of a tetrahedral or triangular mesh).

Reduce the number of phases.

You may find that even a very simple approximation will provide you with useful information about

your problem.

See Eulerian Model (p. ) and Setting Solution Limits (p. ) for more solution strategies for Eulerian

interaction for an Eulerian multiphase calculation are provided below.

The procedure for defining the primary phase in an Eulerian multiphase calculation is the same as

for a VOF calculation. See Defining the Primary Phase (p. ) for details.

To define a non-granular (that is, liquid or vapor) secondary phase in an Eulerian multiphase calculation,

Box for a Non-Granular Phase (p. )).

Figure . : The Secondary Phase Dialog Box for a Non-Granular Phase

Setting Up the Eulerian Model

the material properties for the primary phase (see Defining the Primary Phase (p. )).

. In the Properties group box, specify the Diameter of the bubbles or droplets of this phase.You can

specify a constant value, or use a user-defined function. See the Fluent Customization Manual for details

about user-defined functions.

To define a granular (that is, particulate) secondary phase in an Eulerian multiphase calculation, perform

Box for a Granular Phase (p. )).

Figure . : The Secondary Phase Dialog Box for a Granular Phase

Important

(UDFs).

. (optional) Enable the Packed Bed option if you want to freeze the velocity field for the granular phase.

Note that when you select the packed bed option for a phase, you should also use the fixed velocity

option with a value of zero for all velocity components for all interior cell zones for that phase. Using

fixed velocity in radial direction as a constant value (other than zero) does not ensure continuity.With

the fixed velocity option, both velocity and pressure are fixed in a zone. Since face area in the radial dir-

ection is a function of radial distance from the axis, it will result in a mass conservation problem due to

flux imbalance.

Using zero fixed velocity in the radial direction does not cause any problems related to mass

conservation.

. Specify the Granular Temperature Model. Choose either the default Phase Property option or the

Partial Differential Equation option. See Granular Temperature in the Theory Guide for details.

Diameter

(Equation . ), or gidaspow (Equation .) will use these expressions for the kinetic portion

of the viscosity and will calculate the collisional portion of the viscosity from Equation . in the

Fluent Theory Guide. Alternatively, you can select user-defined to use a user-defined function. Note

that if you select user-defined, your user-defined function must include both the kinetic portion

and the collisional portion of the viscosity in the value it returns.

specifies the solids bulk viscosity (

in Equation . in the Theory Guide).You can select constant

(the default) in the drop-down list and specify a constant value, select lun-et-al to compute the value

using Equation . in the Theory Guide, or select user-defined to use a user-defined function.

specifies a shear viscosity based on the viscous-plastic flow (

Guide). By default, the frictional viscosity is neglected, as indicated by the default selection of none

in the drop-down list. If you want to include the frictional viscosity, you can select constant and

specify a constant value, select schaeffer to compute the value using Equation . in the Theory

Guide, or select user-defined to use a user-defined function.

Angle of Internal Friction

specifies a constant value for the angle  used in Schaeffer’s expression for frictional viscosity

(Equation . in the Theory Guide).This parameter is relevant only if you have selected schaeffer

or user-defined for the Frictional Viscosity.

(.)

with

value is ..

specifies the solids granular conductivity (

value is ..

in Equation . in the Theory Guide).You can select

syamlal-obrien to compute the value using Equation . in the Theory Guide, select gidaspow

to compute the value using Equation . in the Theory Guide, or select user-defined to use a

user-defined function. Note that in the algebraic model, shown in Figure . :The Secondary Phase

Dialog Box for a Granular Phase (p. ), the granular conductivity is not required in the computation

of the granular temperature.This has been obtained by neglecting convection and diffusion in the

transport equation, Equation . in the Theory Guide [] (p. ).

motion of the particles. Choose the algebraic, constant, dpm-averaged, or user-defined option.

Note

The dpm-averaged method is only available when using the Dense Discrete Phase

Model (DDPM).

the lun-et-al, the syamlal-obrien, the ma-ahmadi, none, or a user-defined option.

(.)

with

.

(.)

with

.

.... Defining the Interfacial Area Concentration

When using the Eulerian multiphase model, you can choose to solve a transport equation for the in-

terfacial area, which allows for a distribution of secondary phase diameter, or you can use an algeb-

raic model to compute the interfacial area from a specified diameter. To use an algebraic model, refer

to Using an Algebraic Interfacial Area Model (p. ). To solve the transport equation (Interfacial Area

Concentration in the Fluent Theory Guide), perform the following steps:

Diameter

Diameter

Hibiki-Ishii Model

alpha_max

alpha_max

alpha_max

alpha_max

Guide.

phase.You can choose from constant or user-defined. If the Boiling Model option is enabled, you

can also select yao-morel.The yao-morel option is described in Yao-Morel Model in the Theory

Guide.

(.)

where

and

where

,

,

, and

meter.

allow you to specify the minimum and maximum diameters of the secondary phase to which the

interfacial area concentration model is applied, preventing some computing anomalies to spread

beyond control.

Note

Note

.... Defining the Interaction Between Phases

For both granular and non-granular flows, you will need to specify the drag function to be used in

the calculation of the momentum exchange coefficients. You can also specify lift forces, wall lubrication

forces (for non-granular flows only), turbulent dispersion forces, surface tension effects, and virtual

mass force. For granular flows, you will also need to specify the restitution coefficient(s) for particle

To specify these parameters, click Interaction... to open the Phase Interaction Dialog Box (p. ) and

visit the Drag, Lift, Wall Lubrication, Turbulent Dispersion, Collisions, and Surface Tension tabs.

..... Specifying the Drag Function

ANSYS Fluent allows you to specify a drag function for each pair of phases. Perform the following

steps:

. Click the Drag tab.

. For each pair of phases, select the appropriate drag function from the corresponding drop-down list.

steps:

Select ishii to use the fluid-fluid drag function described by Equation . in the Theory Guide.

This option is available when the boiling model is enabled.

Select schiller-naumann to use the fluid-fluid drag function described by Equation . in the

Theory Guide.The Schiller and Naumann model is the default method, and it is acceptable for general

use in all fluid-fluid multiphase calculations.When using the homogeneous population balance

models you can also select schiller-naumann-pb in which case the interfacial area will be calculated

directly from the population balance variables.

Select morsi-alexander to use the fluid-fluid drag function described by Equation . in the

Theory Guide.The Morsi and Alexander model is the most complete, adjusting the function definition

frequently over a large range of Reynolds numbers, but calculations with this model may be less

stable than with the other models.

Select symmetric to use the fluid-fluid drag function described by Equation . in the Theory

Guide.The symmetric model is recommended for flows in which the secondary (dispersed) phase in

one region of the domain becomes the primary (continuous) phase in another. For example, if air is

injected into the bottom of a container filled halfway with water, the air is the dispersed phase in the

bottom half of the container; in the top half of the container, the air is the continuous phase.The

symmetric drag law is the default method for the Multi-Fluid VOF Model, which is available with

Eulerian multiphase model.

Select grace to use the fluid-fluid drag function described by Equation . in the Theory

Guide. The Grace model is recommended for gas-liquid flows in which the bubbles can have

a range of shapes such as spherical, elliptical, or cap.

In the Grace Swarm Correction dialog box that opens automatically when you first select this

model, you can specify Coefficient: Cexp (

as constant or user-defined. Depending on the flow regime and the bubble size, the following

values should be used:

– Sparsely distributed fluid particles

In flows with sparsely distributed fluid particles,

Guide is zero (default).

– Densely distributed fluid particles

→ Since small bubbles tend to rise slowly in high gas volume fractions due to an increase in the

effective mixture viscosity, a negative

should be used.The Ishii-Zuber correlation uses an

exponent of - for this limit. A value of -. has also been used successfully by some investigators.

→ Large bubbles, on the other hand, tend to rise faster at high gas volume fractions because they

are dragged along by the wakes of other bubbles.This is modeled by using a positive

.The

Ishii-Zuber correlation uses an exponent of  for this regime. A value of  has also been used

successfully by some researchers in the past

See Grace et al. Model in the Fluent Theory Guide for more information.

Select tomiyama to use the fluid-fluid drag function described by Equation . in the

Theory Guide. Like the Grace model, the Tomiyama model is recommended for gas-liquid flows

in which the bubbles can have a range of shapes such as spherical, elliptical, or cap.

Select ishii-zuber to use the fluid-fluid drag function described in Ishii-Zuber Drag Model in the Fluent

Theory Guide.The model automatically accounts for swarms of bubbles moving together in high gas

volume fractions. Like the Grace and Tomiyama drag models, the Ishii-Zuber drag law is recommended

for gas-liquid flows in which bubbles may have a range of shapes such as spherical, elliptical, or cap.

Select anisotropic to use the fluid-fluid drag function described in Multi-Fluid VOF Model in the

Theory Guide.The anisotropic drag law is recommended for free surface modeling. It is based on

higher drag in the normal direction to the interface and lower drag in the tangential direction to the

Select universal-drag for bubble-liquid and/or droplet-gas flow when the characteristic length

of the flow domain is much greater than the averaged size of the droplets/bubbles. It is suitable

for flows in which the bubbles/droplets may have a range of shapes. The universal drag law

is described using Equation . in the Theory Guide. When universal-drag is selected, you

will need to set a value for the surface tension coefficient, under the Surface Tension tab, in

the Phase Interaction dialog box. This value will apply to the primary phase and the secondary

phase.

Select wen-yu to use the fluid-solid drag function described by Equation . in the Theory Guide.

The Wen and Yu model is applicable for dilute phase flows, in which the total secondary phase volume

fraction is significantly lower than that of the primary phase.When using the homogeneous population

balance models you can also select wen-yu-pb in which case the interfacial area will be calculated

Select gidaspow to use the fluid-solid drag function described by Equation . in the Theory

Guide.The Gidaspow model is recommended for dense fluidized beds.

Select syamlal-obrien to use the fluid-solid drag function described by Equation . in the Theory

Guide.The Syamlal-O’Brien model is recommended for use in conjunction with the Syamlal-O’Brien

model for granular viscosity.

Select syamlal-obrien-para to use the parameterized formulation of the Syamlal-O’Brien model de-

scribed by Equation . in the Theory Guide. This model addresses under/over-prediction of bed

expansion that can arise with syamlal-obrien.When you first select this model, you will be presented

with the Syamlal Obrien Model dialog box.

Figure . : Syamlal Obrien Model Dialog Box

There are two inputs:

Void Fraction

the volume fraction of the gas phase in the bed at the minimum fluidization condition

Minimum Fluidization Velocity

the expected or experimentally-determined nominal minimum fluidization velocity of the gas

phase

Once you have input these values, click Validate/Apply to compute the coefficients c1 and

d1 used in Equation . in the Fluent Theory Guide. A message will also be printed to the

text user interface summarizing the fluid and flow properties used in the computation and the

resulting values. You should check that these property values are consistent with the properties

set elsewhere.

Important

If you change property values in the Create/Edit Materials dialog box or dia-

Important

meter in the Secondary Phase dialog box, you must initialize the flow field or

run at least one iteration before computing c1 and d1. Otherwise, incorrect

properties will be used in the computation.

Note that the syamlal-obrien-para model is appropriate only for Geldart Group

B particles and is only applicable to cases involving a single secondary phase.

Select syamlal-obrien-symmetric to use the solid-solid drag function described by Equation .

in the Theory Guide.The symmetric Syamlal-O’Brien model is appropriate for a pair of solid phases.

Select huilin-gidaspow to use the fluid-solid drag function described by Equation . in the

Theory Guide.This option provides a better blending function for the Gidaspow model when moving

from the dense packing limit to the dilute flow limit.

Select gibilaro to use the fluid-solid drag function described by Equation . in the Theory Guide.

This option is used for circulating fluidized beds

Select constant to specify a constant value for the drag function, and then specify the value in the

text field.

Select user-defined to use a user-defined function for the drag function (see the Fluent Customization

Manual for details).

If you want to temporarily ignore the interaction between two phases, select none.

...... Drag Modification

When using the Eulerian or Mixture multiphase models, you can optionally specify a drag modification

term for the selected drag law. The drag modification term acts as a multiplier for the drag coefficient

computed from the models detailed in Specifying the Drag Function (p. ). You can specify the

drag modification term individually for each pair of primary-secondary phases. To enable drag

modification, perform the following steps:

. Check Drag Modification in the Drag tab of the Phase Interaction dialog box.

An additional drop-down list will appear under Drag Factor for each primary-secondary phase

pair.

. For each pair of phases, select the Drag Factor to use from the drop-down list.

Select none to use the selected drag model without modification.

Select constant to specify a constant value for the drag modification factor.

Select brucato to use the Brucato et al. correlation described by Brucato et al. Correlation in the

Select user-defined to use a user-defined function for the drag modification factor (see

DEFINE_EXCHANGE_PROPERTY in the Fluent Customization Manual for details).

For additional details on the implementation of the drag modification, see Drag Modification in the

..... Specifying the Restitution Coefficients (Granular Flow Only)

For granular flows, you need to specify the coefficients of restitution for collisions between particles

(

in Equation . in the Theory Guide). In addition to specifying the

restitution coefficient for collisions between each pair of granular phases, you will also specify the

restitution coefficient for collisions between particles of the same phase.

Perform the following steps:

. Click the Collisions tab to display the Restitution Coefficient inputs.

. For each pair of phases, specify a constant restitution coefficient. All restitution coefficients are equal

to . by default.

..... Including the Lift Force

For both granular and non-granular flows, it is possible to include the effect of lift forces (

in

Equation . in the Theory Guide) on the secondary phase particles, droplets, or bubbles. These

lift forces act on a particle, droplet, or bubble mainly due to velocity gradients in the primary-phase

flow field. In most cases, the lift force is insignificant compared to the drag force, so there is no

reason to include it. If the lift force is significant (for example, if the phases separate quickly), you

may want to include this effect.

Important

Note that the lift force will be more significant for larger particles, but the ANSYS Flu-

ent model assumes that the particle diameter is much smaller than the interparticle spacing.

Therefore, the inclusion of lift forces is not appropriate for closely packed particles or for

very small particles.

To include the effect of lift forces, perform the following steps:

. Click the Lift tab to display the Lift Coefficient inputs.

. For each pair of phases, select the appropriate specification method from the corresponding drop-down

list. Note that, since the lift forces for a particle, droplet, or bubble are due mainly to velocity gradients

in the primary-phase flow field, you will not specify lift coefficients for pairs consisting of two secondary

phases; lift coefficients are specified only for pairs consisting of a secondary phase and the primary

phase.

Select none (the default) to ignore the effect of lift forces.

Select constant to specify a constant lift coefficient, and then specify the value in the text field.

Select moraga to use the Moraga lift model (Moraga Lift Force Model in the Theory Guide).The

Moraga lift model is applicable to spherical solid particles, drops, and bubbles.

Select saffman-mei to use the Saffman-Mei lift model (Saffman-Mei Lift Force Model in the Theory

Guide).The Saffman-Mei lift model is applicable to spherical solid particles, and to drops and bubbles

that are not significantly distorted.

Select legendre-magnaudet to use the Legendre—Magnaudet lift model (Legendre-Magnaudet Lift

Force Model in the Theory Guide).The Legendre-Magnaudet model is applicable to small diameter

spherical fluid particles, though it can be applied to non-distorted liquid drops and bubbles. It accounts

for momentum transfer between the flow around the particle and the inner recirculation flow inside

the fluid particle caused by fluid friction/stresses at the fluid interface.

Select tomiyama to use the Tomiyama lift model (Tomiyama Lift Force Model in the Theory Guide).

The Tomiyama model is applicable to larger-scale deformable bubbles in the ellipsoidal and spherical

cap regimes. Its main feature is the prediction of the cross-over point in bubble size at which particle

distortion causes a reversal in the sign of the lift force.

Select user-defined to use a user-defined function for the lift coefficient (see the Fluent Customization

..... Including the Wall Lubrication Force

For liquid-gas bubbly flows using the Eulerian multiphase model, you can include the effect of wall

lubrication forces (

in Equation . in the Theory Guide) on the secondary phase bubbles.

These forces tend to push the bubbles away from walls at small wall distances. For details on how

wall lubrication is modeled in ANSYS Fluent see Wall Lubrication Force in the Theory Guide.

To include the effect of wall lubrication forces, perform the following steps:

. Click the Wall Lubrication tab to display the Wall Lubrication inputs.

list. Note that you will specify the wall lubrication only for pairs consisting of a secondary phase and

the primary phase.

Select none (the default) to ignore the effect of wall lubrication forces.

Select antal-et-al to use the Antal et al. model (Antal et al. Model in the Theory Guide).You can edit

the model parameters in the Antal Model dialog box (Figure . : Antal et al. Model Dialog

Box (p. )).

Figure . : Antal et al. Model Dialog Box

The following model parameters are available:

Coefficient: Cw1

Specify the constant

in Equation . in the Theory Guide.You can enter a constant value

or specify a user-defined function defined using the DEFINE_EXCHANGE_PROPERTY macro

(DEFINE_EXCHANGE_PROPERTY).

Coefficient: Cw2

Select tomiyama to use the Tomiyama model (Tomiyama Model in the Theory Guide).This model is

only applicable for pipe geometries.You can enter the Hydraulic Diameter for your geometry in the

Tomiyama Model dialog box (Figure . :Tomiyama Model Dialog Box (p. )).

Figure . : Tomiyama Model Dialog Box

Hydraulic Diameter: D (m)

Specify the hydraulic diameter,

, in Equation . in the Theory Guide.

Important

The hydraulic diameter must be entered in units of meters.

Select frank to use the Frank et al. model (Frank Model in the Theory Guide).You can edit the model

parameters in the Frank Model dialog box (Figure . : Frank Model Dialog Box (p. )).

Figure . : Frank Model Dialog Box

Coefficient: Cwc

Specify the cutoff coefficient,

, in Equation . in the Theory Guide.You can enter a constant

value or specify a user-defined function defined using the DEFINE_EXCHANGE_PROPERTY

macro (DEFINE_EXCHANGE_PROPERTY).

Coefficient: Cwd

Specify the damping coefficient,

, in Equation . in the Theory Guide.You can enter a

constant value or specify a user-defined function defined using the DEFINE_EXCHANGE_PROP-

ERTY macro (DEFINE_EXCHANGE_PROPERTY).

Power-law Index: m

Specify the power law constant,

Select hosakawa to use the Hosokawa model (Hosokawa Model in the Theory Guide).You can edit

the model parameters in the Hosokawa Model dialog box (Figure . : Hosokawa Model Dialog

Box (p. )).

Figure . : Hosokawa Model Dialog Box

Formulations

Select which formulation of the Hosokawa model to use.You can select either Frank or Tomiyama.

Hosokawa Coefficient

Specify the coefficient of the Eotvos number in Equation . in the Theory Guide.You can

enter a constant value or specify a user-defined function defined using the DEFINE_EX-

CHANGE_PROPERTY macro (DEFINE_EXCHANGE_PROPERTY).

Coefficients

Specify the model parameters associated with the formulation you selected under Formulations.

Select user-defined to use a user-defined function for the wall lubrication coefficient (see

..... Including the Turbulent Dispersion Force

For turbulent flows using the Eulerian multiphase model, you can include the effects of turbulent

dispersion force (

in Equation . in the Theory Guide). The turbulent dispersion force acts as

a turbulent diffusion in dispersed flows. For details on how turbulent dispersion is modeled in ANSYS

Fluent see Turbulent Dispersion Force in the Theory Guide.

To include the effects of turbulent dispersion force, perform the following steps:

. Click the Turbulent Dispersion tab to display the Turbulent Dispersion inputs.

list. Note that you will specify the turbulent dispersion only for pairs consisting of a secondary phase

and the primary phase.

Select none (the default) to ignore the effects of turbulent dispersion.

Select lopez-de-bertodano to use the Lopez de Bertodano model (Lopez de Bertodano Model in

the Theory Guide).You can edit the model parameters in the Lopez de Bertodano Model dialog

box (Figure . : Lopez de Bertodano Model Dialog Box (p. )).

Figure . : Lopez de Bertodano Model Dialog Box

Model Constant

Specify the coefficient,

Limiting Function

Specify the limiting function to use.You may select none, the standard limiting function, or a

user-defined function using the DEFINE_EXCHANGE_PROPERTY macro (DEFINE_EX-

CHANGE_PROPERTY). See Limiting Functions for the Turbulent Dispersion Force in Fluent Theory

Guide for details on the limiting functions.

Select simonin to use the Simonin model (Simonin Model in the Theory Guide).

You can specify the model parameters in the Simonin Model dialog box (Figure . : Simonin

Figure . : Simonin Model Dialog Box

Select burns-et-al to use the Burns et al. model (Burns et al. Model in the Theory Guide).You can

edit the model parameters in the Burns-et-al Model dialog box (Figure . : Burns et al. Model

Figure . : Burns et al. Model Dialog Box

Select diffusion-in-vof to use the Diffusion in VOF model (Diffusion in VOF Model in the Theory

Guide).You can edit the model parameters in the Diffusion-in-vof Model dialog box (Figure . : Dif-

fusion—in—vof Model Dialog Box (p. )).

Figure . : Diffusion—in—vof Model Dialog Box

VOF Diffusion Coefficient

Select user-defined to use a user-defined function for the turbulent dispersion (see DEFINE_VEC-

TOR_EXCHANGE_PROPERTY in the Fluent Customization Manual for details).

..... Including Surface Tension and Wall Adhesion Effects

or We

.

Important

Note that the calculation of surface tension effects will be more accurate if you use a

quadrilateral or hexahedral mesh in the area(s) of the computational domain where surface

tension is significant. If you cannot use a quadrilateral or hexahedral mesh for the entire

domain, then you should use a hybrid mesh, with quadrilaterals or hexahedra in the af-

fected areas. ANSYS Fluent also offers an option to use VOF gradients at the nodes for

curvature calculations on meshes when more accuracy is desired. For more information,

see Surface Tension and Adhesion in the Theory Guide.

of phases, as described in Surface Tension and Adhesion in the Theory Guide, refer to Including

Surface Tension and Adhesion Effects (p. ).

..... Including the Virtual Mass Force

For both granular and non-granular flows, it is possible to include the “virtual mass force” (

in

Equation . in the Theory Guide) that is present when a secondary phase accelerates relative

to the primary phase. The virtual mass effect is significant when the secondary phase density is much

smaller than the primary phase density (for example, for a transient bubble column).

To include the effect of the virtual mass force perform the following steps:

.

Click the Virtual Mass tab to display the Virtual Mass inputs.

.

Enable Virtual Mass Modeling.

.

For each phase pair listed under Virtual Mass Coefficient, select the method for specifying the virtual

mass coefficient,

, in Equation . in the Fluent Theory Guide.You can choose from the following

methods:

none

Disable virtual mass modeling for the phase pair.

constant

Specify a constant value for the coefficient.The default value of . is typical.

Use a user-defined function created with the DEFINE_EXCHANGE_PROPERTY macro. See

DEFINE_EXCHANGE_PROPERTY in the Fluent Customization Manual for details.

Important

No virtual mass effects will be included unless the Virtual Mass Modeling option is

enabled.

.

If desired, you can enable the Implicit method for virtual mass.

When using the Implicit method, the Default option uses the complete term in Equation ..

enabled.

.

You can also choose Option  or Option , which use locally truncated forms of the virtual

mass terms in cells where divergence is detected.

The Implicit method is recommended for steady-state coupled simulations as it offers improved

convergence in such cases. The recommended approach is to begin the simulation using Option

. Once the solution has converged enough to establish the basic flow field, switch back to

Default to include the complete virtual mass term.

If you are using the Eulerian model to solve a turbulent flow, you will need to choose one of turbulence

models described in Turbulence Models in the Theory Guide in the Viscous Model Dialog Box (p. )

(Figure . : The Viscous Model Dialog Box for an Eulerian Multiphase Calculation (p. )).

Figure . : The Viscous Model Dialog Box for an Eulerian Multiphase Calculation

. Select k-epsilon, k-omega, or Reynolds Stress under Model.

. Select the desired k-epsilon Model, k-omega Model, or Reynolds-Stress Model and any other related

parameters, as described for single-phase calculations in Steps in Using a Turbulence Model (p. ).

. Under Turbulence Multiphase Model or RSM Multiphase Model, indicate the desired multiphase tur-

bulence model (see Turbulence Models in the Theory Guide for details about each):

Select Mixture to use the mixture turbulence model.This is the default model.

Select Dispersed to use the dispersed turbulence model.This model is applicable when there is clearly

one primary continuous phase and the rest are dispersed dilute secondary phases.

Select Per Phase to use a -  or -

turbulence model for each phase.This model is appropriate

when the turbulence transfer among the phases plays a dominant role.

.... Including Turbulence Interaction Source Terms

By default, interphase turbulence source terms are not included in the calculation. If you want to in-

clude these source terms, you can enable them from the Turbulence Interaction tab of the Phase

Interaction Dialog Box (p. ).

. Click the Interaction... button to open the Phase Interaction dialog box (for example, Figure . :The

Phase Interaction Dialog Box for Turbulence Interaction (p. )).

Figure . : The Phase Interaction Dialog Box for Turbulence Interaction

. Click the Turbulence Interaction tab in the Phase Interaction dialog box.

. For each pair of phases, select the desired correlation for the Turbulence Interaction.The available options

are:

select none to omit turbulence interaction source terms.This is the default.

select troshko-hassan to use the Troshko-Hassan model described in Troshko-Hassan in the Fluent

Theory Guide.You can edit the model parameters in the Troshko-Hassan Model dialog box (Fig-

ure . :Troshko-Hassan Model Dialog Box (p. )).

Figure . : Troshko-Hassan Model Dialog Box

Coefficient: Cke

, in the equations in Troshko-Hassan in the Fluent Theory Guide.

Coefficient: Ctd

select sato to use the Sato model described in Sato in the Fluent Theory Guide.You can edit the model

parameters in the Sato Model dialog box (Figure . : Sato Model Dialog Box (p. )).

Figure . : Sato Model Dialog Box

Model Coefficient

, in the equations in Sato in the Fluent Theory Guide.

select simonin-et-al to use the Simonin et al. model described in Simonin et al. in the Fluent Theory

Guide.This option is available only when Dispersed or Per Phase is selected in the Viscous Model

dialog box.You can edit the model parameters in the Simonin-et-al Model dialog box (Figure . : Si-

monin-et-al Model Dialog Box (p. )).

Figure . : Simonin-et-al Model Dialog Box

Drift Turbulent Source

include the portion the turbulent kinetic energy source term arising from the drift velocity.

, in the equations in Simonin et al. in the Fluent Theory Guide.

If you decide to enable turbulence interaction for multiple phase pairs, it is recommended that you

avoid mixing the different models and that you select the same model for each phase pair with tur-

bulence interaction enabled.

Note that the inclusion of these terms can slow down convergence noticeably. If you are looking for

additional accuracy, you may want to compute a solution first without these sources, and then con-

tinue the calculation with these terms included. In most cases these terms can be neglected.

.... Customizing the k- ε Multiphase Turbulent Viscosity

If you are using the -  multiphase turbulence model, a user-defined function can be used to cus-

tomize the turbulent viscosity for each phase. This option will enable you to modify

in the -

model. For more information, see the Fluent Customization Manual.

In the Viscous Model dialog box, under User-Defined Functions, select the appropriate user-defined

function in the Turbulent Viscosity drop-down list.

To define heat transfer in a multiphase Eulerian simulation, you will need to visit the Phase Interaction

dialog box, after you have enabled the energy equation in the Energy dialog box.

Phase Interaction Dialog Box for Heat Transfer (p. )).

Figure . : The Phase Interaction Dialog Box for Heat Transfer

. Click the Heat tab in the Phase Interaction dialog box.

. Select the desired correlation for the Heat Transfer Coefficient.The available choices will depend upon

what other models you have enabled. Note the following regarding the available choices:

constant-htc

allows you to specify a constant value for the volumetric heat transfer coefficient.

nusselt-number

allows you to specify a value for the Nusselt number from which the heat transfer coefficient will be

computed.

gunn

is frequently used for Eulerian multiphase simulations involving a granular phase.

computed.

gunn

is frequently used for Eulerian multiphase simulations not involving a granular phase.

hughmark

is an extension of Ranz-Marshall to a wider range of Reynolds Number.

tomiyama

is frequently used for Eulerian multiphase simulations of bubbly flows with relatively low Reynolds

number.

none

allows you to ignore the effects of heat transfer between the two phases.

allows you to implement a correlation reflecting a model of your choice, through a user-defined

function.

two-resistance

allows you to independently specify the heat transfer coefficient correlations for the two phases.This

setting is recommended when using the evaporation-condensation mass transfer model.

fixed-to-sat-temp

models heat transfer when all of the heat transfer to a phase interface is used in mass transfer. It as-

sumes that the temperature at the To-Phase in the mass transfer is equal to the saturation temperature.

Note that this model only applies when one of the mass transfer models is enabled.

lavieville-et-al

is only available within the two-resistance formulation and can be used to model the gas-interface

heat transfer coefficient. It assumes that the gas phase retains the saturation temperature by rapid

evaporation or condensation.

is only available within the two-resistance formulation. It may be specified for one phase in which

case that phase temperature is equal to the interfacial temperature.

. Set the appropriate thermal boundary conditions.You will specify the thermal boundary conditions for

each individual phase on most boundaries, and for the mixture on some boundaries. See Cell Zone and

Boundary Conditions (p. ) for more information on boundary conditions, and Eulerian Model (p. )

for more information on specifying boundary conditions for a Eulerian multiphase calculation.

See Description of Heat Transfer in the Theory Guide for more information on heat transfer in the

framework of a Eulerian multiphase simulation and the available models.

If you have chosen not to solve the transport equation for Interfacial Area Concentration (Defining the

Interfacial Area Concentration (p. )), you can select an algebraic model to estimate the interfacial

area from the secondary phase diameter specified in the Secondary Phase Dialog Box (p. ). To choose

an algebraic interfacial area model perform these steps.

the Phase Interaction dialog box (for example, Figure . :The Phase Interaction Dialog Box for Inter-

facial Area (p. )).

Figure . : The Phase Interaction Dialog Box for Interfacial Area

ia-particle

considers only the secondary phase volume fraction in estimating the interfacial area.

considers the volume fraction gradient at the interface between two phases in estimating the interfacial

area.

Additional options are available if you have enabled one of the boiling models. See Including the

area.

Boiling Model (p. ).

See Interfacial Area Concentration in the Fluent Theory Guide for details about the algebraic interfacial

If you are using the Eulerian multiphase model (Setting Up the Eulerian Model (p. )), you have the

option of including the Dense Discrete Phase Model (Dense Discrete Phase Model in the Theory

Guide).

Important

Enabling this model automatically enables the DPM model.You will notice that Interaction

with Continuous Phase in the Discrete Phase Model dialog box is enabled.

The Dense Discrete Phase model is available only with the Eulerian multiphase model.The

limitations that currently apply to DPM and Eulerian multiphase models also apply to the Dense

Discrete Phase model. See Limitations of the Eulerian Model in the Fluent Theory Guide and

Limitations (p. ) for limitations that exist with the DPM and Eulerian multiphase models.

The required work flow when using the dense discrete phase model is as follows:

. Set up the Multiphase Model dialog box (Figure . :The Dense Discrete Phase Model (p. )) to include

the dense discrete phase model parameters.

Setup →

Models →

Figure . : The Dense Discrete Phase Model

a.

Enable Dense Discrete Phase Model under Eulerian Parameters.

b. Set the Number of Discrete Phases that are present in your case.

. Open the Phases dialog box, in order to define the phases.

Edit...

a.

Define the discrete phase, by selecting the phase from the Phases selection list that is labeled Discrete

Edit...

a.

Phase and clicking the Edit... button.Then set up the properties in the Discrete Phase dialog box

that opens, as shown in Figure . :The Discrete Phase Dialog Box (p. ).

Figure . : The Discrete Phase Dialog Box

Note that for non-granular flow, no additional inputs are required here (since the material is

set automatically in the background, and the diameter is part of the solution).

b. To prevent particle concentration from becoming unphysically high, enable Volume Fraction Ap-

proaching Continuous Flow Limit and specify Transition Factor.The criterion of transition from the

standard method to a special treatment is specified as Transition Factor multiplied by the theoretical

close-packing limit for mono-sized spheres (

). If the particle volume fraction exceeds this

transition volume fraction, ANSYS Fluent will apply a special treatment to the particle momentum

equation. For more information, refer to Dense Discrete Phase Model in the Fluent Theory Guide.

The default value for the Transition Factor is ., giving a transition volume fraction of .

(=.*/). Note that the Transition Factor is not limited to a range between  and . In

other words, you can specify values outside this range. For example, a value of . will give a

transition volume fraction of .. You can also specify locally variable values using the

DEFINE_PROPERTY user-defined macro, depending on the local particle size distribution, as

an example.

See DEFINE_PROPERTY UDFs in the Fluent Customization Manual for information about the

DEFINE_PROPERTY.

c.

c.

Define the primary and secondary phases, as described in Defining the Phases for the Eulerian Mod-

el (p. ).

. Define the injections using the Injections dialog box.

New...

a.

Create a new injection by clicking the Create button in the Injections dialog box, or edit an existing

injection by selecting the injection from the Injections list and clicking the Set... button.

b. In the Set Injection Properties dialog box that opens (Figure . :The Set Injection Properties Dialog

Box (p. )), specify properties for each injection as described in Setting Initial Conditions for the

Discrete Phase (p. )

Note

Note that when the DDPM is used, averaged-discrete-phase-drag is automatically

selected for the drag coefficient in the Drag tab of the Phase Interaction dialog

box. averaged-discrete-phase-drag corresponds to

Fluent Theory Guide and indicates that the interaction between discrete and fluid

phases will be computed based on averaged values of fluid drag of all particles

crossing the fluid cell. That is, at each time step, the drag is evaluated for each particle

using the drag law that you have selected in the Set injection Properties dialog

box and then averaged based on the residence time of each particle in the cell.

c.

Select the discrete phase from the Discrete Phase Domain drop-down list.

. Define the material properties for each injection.

Setup →

Materials

.... Defining a Granular Discrete Phase

Setup →

Materials

To define a granular (that is, particulate) discrete phase in an Eulerian multiphase calculation, perform

. Select the phase (for example, Discrete Phase) in the Phases list.

. Click Edit... to open the Discrete Phase dialog box (Figure . :The Discrete Phase Dialog Box for a

Granular Phase (p. )).

Figure . : The Discrete Phase Dialog Box for a Granular Phase

. In the Discrete Phase dialog box, enter a Name for the phase.

. Enable Volume Fraction Approaching Packing Limit to prevent the unlimited accumulation of particles,

which are operating at packing limit conditions.

. Specify the Transition Factor as either a constant or a user-defined function.The default value for the

Transition Factor is ..The transition criterion is based on the local particle volume fraction of the

given discrete phase and is specified as a factor multiplied by the maximum packing limit (also a user-

specified value). For example, for a typical granular phase with a maximum packing limit of ., the

transition volume fraction is the product of . and ., which is equal to ..

You can now define all other fields of the discrete phase in a similar manner to that described in

Defining a Granular Secondary Phase (p. ).

option of including the Boiling Model (see Wall Boiling Models in the Theory Guide).

Note the following limitations:

This model is only available with the Eulerian multiphase model.

This model is only available with the Pressure-Based solver.

The required work flow when using the boiling model is as follows:

. Open the Multiphase Model dialog box (Figure . :The Boiling Model (p. )).

Setup →

Models →

Figure . : The Boiling Model

a.

Enable Boiling Model under Eulerian Parameters.

b. Select RPI Boiling Model, Non-equilibrium Boiling, or Critical Heat Flux as the boiling model option.

Information about the three options is available in RPI Model, Non-equilibrium Subcooled Boiling, and

Critical Heat Flux in the Theory Guide.

c.

Set the total Number of Eulerian Phases that are present in your case.This can consist of two phases:

liquid and vapor, which are directly involved in boiling mass transfer; or it can include “non-boiling

phases” or “species“. If a system consists of three phases: liquid, vapor, and air, then the Number of

Eulerian Phases will be , where air is the non-boiling phase.

Note

To include the liquid volume fraction effects, use the solve/set/multiphase-numer-

ic/boiling-parameters/liquid-vof-factor text command.When this option

is enabled, the heat transfer coefficients of boiling models will be multiplied by the local liquid

volume fraction.

To include the thin film effects, use the solve/set/multiphase-numeric/boiling-

parameters/thin-film text command.When enabled, this option will use Equa-

tion . in the Fluent Theory Guide in the calculation.

. Make sure the energy option is enabled.

Note

Note

The energy option will be automatically turned on when the boiling model is enabled.

On

. Enable Gravity and set the Operating Pressure in the Operating Conditions dialog box.

Important

Make sure gravity is included when the boiling model is used.

. Choose one of the turbulence models that is available with the Eulerian multiphase model.

Setup →

Models →

. Open the Create/Edit Materials dialog box and specify the material properties for the liquid, vapor, solid,

and any other phases that may exist.

Setup →

Materials →

Fluid → Create/Edit...

Important

For the liquid and vapor phases, the Standard State Enthalpy must be specified,

as it is used in the computation of the Latent Heat.

Edit...

Define the liquid as the primary phase by selecting the phase from the Phases selection list that

is labeled Primary Phase and clicking the Edit... button. Define the vapor as the secondary phase.

In the Secondary Phase dialog box, the Diameter is set to boiling-dia by default, but you have

the option of setting it up as a constant value or a user-defined function, as shown in Fig-

ure . : The Secondary Phase Dialog Box (p. ).

Figure . : The Secondary Phase Dialog Box

. Open the Phase Interaction dialog box.

a.

In the Drag tab, select a drag specification method. See Specifying the Drag Function (p. )

a.

for available drag options and their definitions. For boiling flows, ishii is usually chosen.

Figure . : The Phase Interaction Dialog Box

b. In the Lift tab, select moraga, tomiyama, saffman-mei, legendre-magnaudet, or user-defined. For

boiling flows, tomiyama is usually chosen.

c.

In the Wall Lubrication tab, select antal-et-al, tomiyama-et-al, frank, hosokawa, or user-defined

as described in Including the Wall Lubrication Force (p. ). For boiling flows, antal-et-al is typically

chosen.

d. In the Turbulent Dispersion tab, select lopez-de-bertodano, simonin, burns-et-al, diffusion-in-

vof, or user-defined as described in Including the Turbulent Dispersion Force (p. ). For boiling

flows, lopez-de-bertodano is typically chosen.

e. In the Turbulent Interaction tab, select troshko-hassan, sato, or simonin-et-al as described in In-

cluding Turbulence Interaction Source Terms (p. ). For boiling flows, troshko-hassan is typically

chosen.

f.

In the Heat tab, select ranz-marshall, tomiyama, or user-defined. For boiling flows, ranz-marshall

is usually chosen.

g. In the Surface Tension tab, select constant and enter the desired value.

h. In the Interfacial Area tab, you have four formulations available from which to select:

ia-symmetric (see Equation . in the Theory Guide)

ia-particle (see Equation . in the Theory Guide)

ia-ishii (see Equation . in the Theory Guide).This option is only available with the RPI model.

user-defined (see Example - Custom Interfacial Area in the Fluent Customization Manual)

For boiling flows, ia-symmetric or ia-particle are usually chosen.

i.

i.

In the Mass tab, set the Number of Mass Transfer Mechanisms to  and make sure the transfer is

always from the liquid to the vapor phase. Select boiling under Mechanism.The Boiling Model dialog

box will open (Figure . :The Boiling Model Dialog Box (p. )), where you will set the boiling

model parameters and the quenching model corrections.

Figure . : The Boiling Model Dialog Box

i.

Specify the Interfacial Model Constants and the Saturation Temperature.The default values

for the liquid and vapor interface transfer coefficients are .

Note

If you use the polynomial, piecewise-polynomial, or piecewise-linear option

for Saturation Temperature, the pressure-dependency must be specified in

terms of absolute pressure.

If you selected the RPI Boiling Model in the Multiphase Model dialog box, then

you will not need to specify the Vapor-Interface Transfer Coeff., since the vapor

phase temperature is fixed to the saturation temperature.

ii.

Under the Boiling Model Parameters, select the Bubble Departure Diameter that best describes

your model. Five options exist: tolubinski-kostanchuk (the default setting), unal, kocamusta-

faogullari-ishii, constant, and user-defined.The tolubinski-kostanchuk formulation is described

in Equation . in the Theory Guide, the unal formulation is described in Equation . in

the Theory Guide and the kocamustafaogullari-Ishii formulation is described in Equation .

iii. Specify the Frequency of Bubble Departure.You can choose the cole option (which is the default),

or enter a constant value.The cole formulation is described in Equation . in the Theory

Guide.

iv. Specify the Nucleation Site Density.You can choose between lemmert-chawla (which is the

default), kocamustafaogullari-ishii. and user-defined.This quantity is usually represented by a

correlation based on the wall superheat, described in Equation . in the Theory Guide.

Note

It is recommended that when using the kocamustafaogullari-ishii option, it

should be used for both the Bubble Departure Diameter and Nucleation Site

Density.

v.

Specify the Area Influence Coeff. The area of influence is based on the bubble departure diameter

and the nucleate site density, as defined in Equation . in the Theory Guide.You have a choice

of three options when modeling the area of influence coefficient: delvalle-kenning (which is the

default and defined in Equation . in the Theory Guide, constant, and user-defined.

vi. The Quenching Model Correction addresses the quenching term in the wall heat flux partition

(described in Wall Heat Flux Partition in the Theory Guide).The quenching term in the wall heat

flux partition models the cyclic averaged transient energy transfer related to liquid filling the wall

vicinity after the bubble detachment with a period  and it is expressed as:

(.)

where

is the liquid heat conductivity,

is the periodic time, and

is the liquid phase

diffusivity.The Bubble Waiting Time Coefficient,

, is a coefficient introduced to correct the

waiting time between departures of consecutive bubbles.The default value is , however you can

modify this value as needed, but it can only be specified as a constant.

From Equation . (p. ), you can see that the quenching model is strongly dependent

on

, which results in grid-dependent solutions. To remedy this, two approaches have been

adopted in ANSYS Fluent: Fixed Yplus Value and Fixed Liquid Temperature.

Note

When the calculated temperature in regions away from the walls is lower than

the Operating Temperature (set in the Boussinesq Parameters group box in

the Operating Conditions dialog box), the solver uses the operating temperature

for the quenching correction.

vii. Enable the Correction Model if you want to achieve a certain level of grid-independence in your

solution. If this option is disabled, Equation . (p. ) calculates the quench flux term without

corrections.

viii.Select Fixed Yplus Value if you want to use the logarithmic form of the wall functions to estimate

the liquid temperature

at a fixed Yplus value of , as proposed by Egorov and Mentor

[] (p. ), instead of using the liquid temperature values in the near-wall cells. Enter the Minimum

Reference Temperature, which limits the lowest value of the liquid temperature. It should not

be lower than the liquid inlet temperature. Specify a Yplus Value. It is set to  by default.

ix. If you select Fixed Liquid Temperature, you can choose from standard, constant, or user-defined

for the Liquid Reference Temperature.You will also need to enter the Minimum Reference

Temperature.The liquid temperature used to compute the quenching flux should usually be

between the inlet liquid temperature and the saturation temperature.

Note

Note

To learn how to hook boiling parameter user-defined functions, refer to

DEFINE_BOILING_PROPERTY in the Fluent Customization Manual.

. Set up the conditions at inlets, outlets, and thermal conditions for walls.

Setup →

For the quenching wall heat flux, Koncar et al. [] (p. ) have suggested that in order to avoid

grid dependence when calculating the quenching heat transfer, a factor that relates the temperature

at a fixed normalized distance (y+ = ) to the temperature at the near wall cell must be applied.

Contact a technical support engineer for more information.

The wall boiling models are compatible with three different wall boundaries: isothermal wall, spe-

cified heat flux, and specified heat transfer coefficient (coupled wall boundary).

Note

The boiling models do not apply to thin walls.

. Choose Coupled as the pressure-velocity coupling scheme.

Solution →

Methods

Note

Although Phase Coupled SIMPLE is also available, it is generally less robust and is not

recommended for use in steady cases involving boiling or mass transfer.

. The following solution strategies are recommended for boiling model simulations:

Solution →

Controls

Courant Number: use a value between  and  is recommended. As a first try, use a value of

.

Explicit Relaxation Factors: use the default values of  for Momentum and Pressure.

Vaporization Mass: use an under-relaxation factor between . and . As a first try, use a value

of .

Volume Fraction: use an under-relaxation factor between . and ..

of .

Turbulent Kinetic Energy: use an under-relaxation factor between . and ..

Turbulent Viscosity: use an under-relaxation factor between . and ..

Energy: use an under-relaxation factor between . and ..

After you have selected the Eulerian multiphase model (Setting Up the Eulerian Model (p. )), you

can enable the Multi-Fluid VOF Model (Multi-Fluid VOF Model in the Theory Guide).

You cannot use this model with the Dense Discrete Phase Model.

After enabling Multi-Fluid VOF, the Interface Modeling Options become available, as described in

Interface Modeling Type (p. ). You can select from Sharp, Dispersed, or hybrid Sharp/Dispersed

interface modeling to expose the most appropriate discretization schemes for your simulation. You

can also specify some additional time-advancement settings as described in Setting Time-Dependent

Parameters for the Explicit Volume Fraction Formulation (p. ).

The available drag laws depend on your selection for Interface Modeling. Sharp interface modeling

supports only symmetric, anisotropic-drag, user-defined, and none. Sharp/Dispersed interface

modeling supports all the relevant drag laws. Dispersed interface modeling does not support aniso-

tropic-drag, but supports all other relevant drag laws.

Note

Anisotropic drag applicable to free surface modeling is only compatible with the Mixture

turbulence model.

Note

If you want to use the anisotropic drag law, perform the following steps:

. Define the drag law in the Phase Interaction dialog box.

. Click the Drag tab to display the Drag Coefficient inputs.

. For each pair of phases, select the appropriate drag law from the corresponding drop-down list.

Select anisotropic-drag when there is higher drag in the normal direction to the interface and lower

drag in the tangential direction to the interface. For details about this drag law, refer to Multi-Fluid VOF

Model in the Theory Guide.

To specify the input parameters for anisotropic drag, you will need to use the /solve/set/mp-

mfluid-aniso-drag text command. The options for an Anisotropic Drag Method of

(which is based on the symmetric drag), are as follows:

Anisotropic Drag Method

[]

Normal Interfacial Drag Friction Factor

[]

Tangential Interfacial Drag Friction Factor

[]

Length scale

[.]

The options for an Anisotropic Drag Method of  are as follows:

[]

Viscosity option

[]

[]

[]

[.]

. If you have enabled Phase Localized Discretization in the Multiphase Model dialog box, click the Dis-

cretization tab to enable the use of the Phase Localized Compressive Scheme. For information about

applying the various schemes, refer to Discretizing Using the Phase Localized Compressive Scheme (p. ).

.. Setting Up the Wet Steam Model

After you have enabled the density-based solver in ANSYS Fluent, you can choose the wet steam

model (see Wet Steam Model Theory in the Theory Guide) by opening the Multiphase Model dialog

box and selecting the Wet Steam option.

Setup →

Models →

Figure . : The Multiphase Model Dialog Box with the Wet Steam Model Selected

This section includes information about using your own property functions and data with the wet steam

model. Solution settings and strategies for the wet steam model can be found in Wet Steam Mod-

el (p. ). Postprocessing variables are described in Model-Specific Variables (p. ).

... Using User-Defined Thermodynamic Wet Steam Properties

...Writing the User-Defined Wet Steam Property Functions (UDWSPF)

... Compiling Your UDWSPF and Building a Shared Library File

... Loading the UDWSPF Shared Library File

... UDWSPF Example

ANSYS Fluent allows you to use your own property functions and data with the wet steam model. This

is achieved with user-defined wet steam property functions (UDWSPF).

These user-defined functions are written in the C programming language and there is a certain pro-

gramming format that must be used so that you can build a successful library that can be loaded into

The following is the procedure for using the user-defined wet steam property functions (UDWSPF):

. Define the wet steam equation of state and all related thermodynamic and transport property equations.

. Turn on the wet steam model.

. Compile your UDWSPF C functions and build a shared library file using the text user interface.

define → models → multiphase → wet-steam → compile-user-defined-wetsteam-

functions

. Load your newly created UDWSPF library using the text user interface.

define → models → multiphase → wet-steam → load-unload-user-defined-wet-

steam-library

Important

Note that the UDWSPF can only be used when the wet steam model is selected. Therefore,

the UDWSPF are available for use with the density-based solver only.

Creating a UDWSPF C function library is reasonably straightforward:

the definitions for DEFINE macros and other ANSYS Fluent functions to be accessible during the compilation

process.

The code must include at least one in the UDF’s DEFINE functions (that is DEFINE_ON_DEMAND) to be

able to use the compiled UDFs utility.

Any values that are passed to the solver by the UDWSPF or returned by the solver to the UDWSPF are as-

sumed to be in SI units.

You must use the principle set of user-defined wet steam property functions in your UDWSPF library, as

described in the list that follows.These functions are the mechanism by which your thermodynamic

property data is transferred to the ANSYS Fluent solver.

The following lists the user-defined wet steam property function names and arguments, as well as a

short description of their functions. Function inputs from the ANSYS Fluent solver consist of one or

more of the following variables: T = temperature (

), P = pressure (

), and  = vapor-phase density

(

).

void wetst_init(Domain *domain)

This will be called when you load the UDWSPF. You use it to initialize wet steam model constants

or your own model constants. It returns nothing.

real wetst_satP(real T)

Setting Up the Wet Steam Model

This is the saturated pressure function, which takes on temperature in K and returns saturation

pressure in Pa.

real wetst_satT(real P, real T)

This is the saturated temperature function, which takes on pressure in Pa and a starting guess tem-

perature in K and returns saturation temperature in K.

real wetst_eosP(real rho, real T)

This is the equation of state, which takes on vapor density in kg/m3 and Temperature in K and returns

real wetst_eosRHO(real P, real T)

This is the equation of state, which takes on pressure in Pa and temperature in K and returns vapor

density in kg/m3.

real wetst_cpv(real T, real rho)

This is the vapor specific heat at constant pressure, which takes on temperature in K and vapor

density in kg/m3 and returns specific heat at constant pressure in J/kg/K.

real wetst_cvv(real T, real rho)

This is the vapor specific heat at constant volume, which takes on temperature in K and vapor

density in kg/m3 and returns specific heat at constant volume in J/kg/K.

real wetst_hv(real T,real rho)

This is the vapor specific enthalpy, which takes on temperature in K and vapor density in kg/m3 and

returns specific enthalpy in J/Kg.

real wetst_sv(real T, real rho)

This is the vapor specific entropy, which takes on temperature in K and vapor density in kg/m3 and

returns specific entropy in J/Kg/K.

real wetst_muv(real T, real rho)

This is the vapor dynamic viscosity, which takes on temperature in K and vapor density in kg/m3

and returns viscosity in kg/m/s.

real wetst_ktv(real T, real rho)

This is the vapor thermal conductivity, which takes on temperature in K and vapor density in kg/m3

and returns thermal conductivity in W/m/K.

real wetst_rhol(real T)

This is the saturated liquid density, which takes on temperature in K and returns liquid density in

kg/m3.

real wetst_cpl(real T)

This is the saturated liquid specific heat at constant pressure, which takes on temperature in K and

returns liquid specific heat in J/kg/K.

real wetst_mul(real T)

This is the liquid dynamic viscosity, which takes on Temperature in K and returns dynamic viscosity

in kg/m/s.

real wetst_ktl(real T)

This is the liquid thermal conductivity, which takes on temperature in K and returns thermal con-

ductivity in W/m/K.

real wetst_surft(real T)

This is the liquid surface tension, which takes on Temperature in K and returns surface tension N/m.

At the end of the code you must define a structure of type WS_Functions whose members are

pointers to the principle functions listed previously. The structure is of type WS_Functions and its

name is WetSteamFunctionList.

UDF_EXPORT  WS_Functions  WetSteamFunctionList  =

{

{

wetst_init,     /*initialization  function*/

wetst_satP,     /*Saturation  pressure*/

wetst_satT,     /*Saturation  temperature*/

wetst_eosP,     /*equation  of  state*/

wetst_eosRHO,   /*equation  of  state*/

wetst_hv,       /*vapor  enthalpy*/

wetst_sv,       /*vapor  entropy*/

wetst_cpv,      /*vapor  isobaric  specific  heat*/

wetst_cvv,      /*vapor  isochoric  specific  heat*/

wetst_muv,      /*vapor  dynamic  viscosity*/

wetst_ktv,      /*vapor  thermal  conductivity*/

wetst_rhol,     /*sat. liquid  density*/

wetst_cpl,      /*sat. liquid  specific  heat*/

wetst_mul,      /*sat. liquid  viscosity*/

wetst_ktl,      /*sat. liquid  thermal  conductivity*/

wetst_surft     /*liquid  surface  tension*/

};

This section presents the steps you will need to follow to compile your UDWSPF C code and build a

shared library file. This process requires the use of a C compiler. For more details on compiler require-

ments, see Compilers in the Fluent Customization Manual.

Important

To use the UDWSPF you will need to first build the UDWSPF library by compiling your UD-

WSPF C code and then loading the library into the ANSYS Fluent code.

The UDWSPF shared library is built in the same way that the ANSYS Fluent executable itself is built.

Internally, a script called Makefile is used to invoke the system C compiler to build an object code

library that contains the native machine language translation of your higher-level C source code. This

shared library is then loaded into ANSYS Fluent (either at run time or automatically when a case file

is read) by a process called dynamic loading. The object libraries are specific to the computer architecture

level changes, or when the job is run on a different type of computer.

The general procedure for compiling UDWSPF C code is as follows:

. Place the UDWSPF C code in your working directory (that is, where your case file resides).

. Launch ANSYS Fluent.

. Read your case file into ANSYS Fluent.

. You can now compile your UDWSPF C code and build a shared library file using the commands provided

in the text command interface (TUI):

a.

Select the define/models/multiphase/wet-steam menu item.

define → models → multiphase → wet-steam

If the Wet Steam model has not been enabled yet, use the following TUI commands to enable

it:

define/models/multiphase/wet-steam> enable?

Enable wet steam model? [no] yes

b. Select the compile-user-defined-wetsteam-functions option.

c.

Enter the compiled UDWSPF library name.

The name given here is the name of the directory where the shared library (for example, libudf)

will reside. For example, if you press Enter then a directory should exist with the name libudf,

and this directory will contain library file called libudf. If, however, you type a new library

name such as mywetsteam, then a directory called mywetsteam will be created and it will

contain the library libudf.

d. Continue on with the procedure when prompted.

e. Enter the C source file names.

Important

Ideally you should place all of your functions into a single file. However, you can

split them into separate files if desired.

f.

Enter the header file names, if applicable. If you do not have an extra header file, then press Enter

ANSYS Fluent will then start compiling the UDWSPF C code and put it in the appropriate archi-

tecture directory.

To load the UDWSPF library, perform the following steps:

Go to the define/models/multiphase/wet-steam menu item in the text user interface.

Select the load-unload-user-defined-wetsteam-library option and follow the procedure

If the loading of the UDWSPF library is successful, you will see a message similar to the following:

Opening user-defined wet steam library "libudf"...

Library "libudf/lnamd64/2d/libudf.so" opened

Setting material properties to Wet-Steam...

Initializing user defined material properties...

This section describe a simple UDWSPF. You can use this example as the basis for your own UDWSPF

code. For approximate calculations at low pressure, the simple ideal-gas equation of state and constant

isobaric specific heat is assumed and used. The properties at the saturated liquid line and the saturated

vapor line used in this example are similar to the one used by ANSYS Fluent.

/* User Defined Wet Steam Properties:

EOS    : Ideal Gas Eq.

Vapor Sat. Line : W.C.Reynolds tables ()

Liquid Sat. Line: E. Eckert & R. Drake book ()

Use ideal-gas EOS with Steam properties

to model wet steam condensation in low pressure nozzle

Author: L. Zori

Date : Jan.

/

/*Global Constants for this model*/

real ws_TPP = . ;

real ws_aaa = . ;

real cpg = . ;/* Cp-vapor at low-pressure region*/

{

}

{

/*

You must initialize these material property constants.

they will be used in the wet steam model in fluent

/

ws_Tc = . ;/*Critical Temp. */

ws_Pc = . ;/*Critical Pressure */

mw_f  = . ;/*fluid droplet molecular weight (water) */

Rgas_v  = . ;/*vapor Gas Const*/

}

{

real psat;

real SUM=. ;

real pratio;

real F;

real a1 = -. ;

real a2 = .97210000E-;

real a3 = -.15528600E-;

real a4 = .68563500E-;

real a5 = .09409899E-;

real a6 = -.39993000E-;

real a7 = .52065800E-;

real a8 = -.21868400E-;

if (T > ws_Tc) T = ws_Tc ;

F  = ws_aaa*(T - ws_TPP)  ;

SUM = a1 + F*(a2+ F*(a3+ F*(a4+ F*(a5+ F*(a6+ F*(a7+ F*a8)))))) ;

pratio = (ws_Tc/T - . )*SUM;

psat  = ws_Pc *exp(pratio) ;

return psat; /*Pa */

}

real

wetst_satT(real P, real T)

{

real tsat;

real dT, dTA,dTM,dP,p1,p2,dPdT;

real dt = .e-;

int i ;

for (i=; i<; ++i)

{

if (T > ws_Tc) T = ws_Tc-. ;

p1= wetst_satP(T)  ;

p2= wetst_satP(T+dt) ;

{

real tsat;

int i ;

{

dPdT = (p2-p1)/dt;

dP = P - p1 ;

dT = dP/dPdT  ;

dTA = fabs(dT);

T = T + dT;

if (fabs(dT)<TEMP_eps*T) break;

}

tsat = T;

return tsat; /*K */

}

real

wetst_eosP(real rho, real T)

{

real P;

P = rho* Rgas_v * T ;

return P; /*Pa */

}

real

wetst_eosRHO(real P, real T)

{

real rho;

rho = P/(Rgas_v * T) ;

return rho; /*kg/m3 */

}

real

wetst_cpv(real T, real rho)

{

real cp;

cp = cpg ;

return cp; /* (J/Kg/K) */

}

real

wetst_cvv(real T, real rho)

{

real cv;

cv = wetst_cpv(T,rho) - Rgas_v ;

return cv; /* (J/Kg/K) */

}

real

wetst_hv(real T,real rho)

{

real h;

h = T* wetst_cpv(T,rho) ;

return h; /* (J/Kg) */

}

real

wetst_sv(real T, real rho)

{

real s ;

real TDatum=. ;

real PDatum=.01325e5;

s=wetst_cpv(T,rho)*log(T/TDatum)+

Rgas_v*log(PDatum/(Rgas_v*T*rho));

return s; /* (J/Kg/K) */

}

real

wetst_muv(real T, real rho)

{

real muv;

muv=.7894e- ;

return muv; /* (Kg/m/s) */

}

real

wetst_ktv(real T, real rho)

{

real ktv;

ktv=. ;

return ktv; /* W/m/K */

}

real

wetst_rhol(real T)

{

real rhol;

real SUM = . ;

int ii;

int i;

real rhoc = . ;

real D[];

D[] =  . ;

D[] = -.8512396E+ ;

D[] =  .2265240E+ ;

D[] = -.8243852E+ ;

D[] =  .0002765E+ ;

D[] = -.6122557E+ ;

D[] =  .8297674E+ ;

D[] = -.3350520E+ ;

for(ii=;ii ;++ii)

{

i = ii+ ;

SUM += D[ii] * pow((. - T/ws_Tc), i/. );

}

rhol = rhoc*(.+SUM);

return rhol; /* (Kg/m3) */

}

real

wetst_cpl(real T)

{

real cpl;

real a1= -. ;

real a2= . ;

real a3= -. ;

real a4= . ;

}

}

real

{

real cpl;

real a2= . ;

real a4= . ;

real a5= -.00561e-;

real a6= .14336E-;

cpl = a1 + T*(a2+ T*(a3+ T*(a4+ T*(a5+ T*a6)))) ;

return cpl; /* (J/Kg/K) */

}

real

wetst_mul(real T)

{

real mul;

real a1= . ;

real a2= -. ;

real a3= .16604E- ;

real a4= -.26258E-;

real a5= .13969E-;

real a6= -.92145E-;

real a7= .14092E-;

mul = a1 + T*(a2+ T*(a3+ T*(a4+ T*(a5+ T*(a6+ T*a7))))) ;

return mul; /* (Kg/m/s) */

}

real

wetst_ktl(real T)

{

real ktl;

real a2= . ;  real a3= .48603E-;

real a4= -.31689E-;

real a5= .47590E-;

real a6= -.55638E-;

ktl = a1 + T*(a2+ T*(a3+ T*(a4+ T*(a5+ T*a6)))) ;

return ktl; /* W/m/K */

}

real

wetst_surft(real T)

{

real sigma;

real Tr;

real a1= . ;

real a2= . ;

real a4= . ;

Tr  = T/ws_Tc ;

sigma = . *(a1 + Tr*(a2+ Tr*(a3+ Tr*a4))) ;

return sigma ;/* N/m */

}

/* do not change the order of the function list */

UDF_EXPORT WS_Functions WetSteamFunctionList =

{

};

.. Solution Strategies for Multiphase Modeling

Important

... Coupled Solution for Eulerian Multiphase Flows

... Coupled Solution for VOF and Mixture Multiphase Flows

Solution Strategies for Multiphase Modeling

... Selecting the Pressure-Velocity Coupling Method

... Controlling the Volume Fraction Coupled Solution

...VOF Model

... Mixture Model

... Eulerian Model

...Wet Steam Model

In multiphase flow, the phasic momentum equations, the shared pressure, and the phasic volume

fraction equations are highly coupled. Traditionally, these equations have been solved in a segregated

fashion using some variation of the SIMPLE algorithm to couple the shared pressure with the momentum

equations. This is attained by effectively transforming the total continuity into a shared pressure. The

ANSYS Fluent  Phase Coupled SIMPLE algorithm has been successfully implemented and solves a

wide range of multiphase flows. However, coupling the linearized system of equations in an implicit

manner would offer a more robust alternative to the segregated approach.

One of the fundamental problems is that the resulting matrix is not symmetric and that the continuity

constraint may contribute to a zero diagonal block, making the solution difficult to obtain. One way

to circumvent this problem is to use direct solvers, but these are too expensive for large industrial

cases. In addition, we need to avoid a zero diagonal, resulting from the continuity constraint, and like

the segregated solver, we need to construct a pressure correction equation. In multiphase, we also

have the additional problem of the vanishing phase, which for the coupled solver is important to ensure

some continuity in the coefficients. Like the Phase Coupled, we use a Rhie and Chow type of scheme

to calculate volume fluxes and to provide proper coupling between velocity and pressure, thereby

avoiding unphysical oscillations.

Consider a single-phase system and let us denote the velocity correction components in the three

Cartesian directions by

,

, and

with

denoting the shared pressure correction. These are discrete

variables and can be expressed in the form

. The linear system that is generated by the single-

phase coupled solver is of the form

(.)

For a notation in component form

(.)

Now let us consider a multiphase system of n-phases and denote the phasic velocity correction com-

ponents in the three Cartesian directions by

,

, and

where the subscript  represents the phase

notation,

denotes the shared pressure correction and

denotes the volume fraction correction

,

, and

notation,

(ANSYS Fluent can solve in both correction form for velocity and volume fraction and non-correction

form). For simplicity the matrix will be shown for two phases. The vector solution is of the form

or in a shorter notation

. The linear system would be an ex-

tension of the one generated by the coupled solver shown by Equation . (p. ).

(.)

This system can be easily generalized to  phases. The components of this matrix are also matrices.

For large problems we need to resort to iterative solvers. The ANSYS Fluent AMG Coupled solver with

an ILU smoother has proved to be a robust method. Most coupled solvers also need a pseudo stepping

method, adding more diagonal dominance to the matrix. Our method here is to use under-relaxation

factors for momentum, which is equivalent to time stepping in steady flows. Similar to that of the

single phase, we have introduced a steady Courant Number instead of an under-relaxation for velocities.

Having this control is important when using second order numerical schemes in the convective terms.

For the sake of simplicity, input parameters for the Coupled solver are similar to the single-phase

solver. We have the options for solving the whole system including volume fraction, or to treat the

volume fraction solution in a segregated manner while preserving the pressure-velocity coupling for

all phases.

Important

Equations in multiphase are more strongly linked than single phase and generally may need

more under-relaxation, hence using the same values as single phase may not be ideal. A

Important

low Courant number would stabilize the solution.

See Selecting the Pressure-Velocity Coupling Method (p. ) for information about applying the various

algorithms.

We have the option of solving the multiphase system for VOF and mixture multiphase models in the

following ways:

Solving the continuity and momentum equations in a coupled manner (see Coupled Algorithm in the

Theory Guide) and solving the volume fraction equation in a segregated manner.

Solving the volume fraction equation in a coupled manner along with the continuity and momentum

equations.

Solving the volume fraction equation in a coupled manner requires discretization of the volume fraction

equation in the correction form along with the discretization of the continuity and momentum equation,

as discussed in Coupled Algorithm in the Theory Guide.

The volume fraction equation could be represented in the discretized form as

(.)

The overall system of equations after being transformed to the correction form could be represented

as

(.)

For a 2D case and two-phase flow, the system could be expanded as follows:

(.)

and the unknown and residual vectors have the form

(.)

(.)

where

= coefficient matrix

= solution vector

= residual vector

= pressure correction

= velocity corrections

= volume fraction correction

The settings that are available in the Solution Methods task page (see Figure . : The Solution

Methods Task Page Displaying The Pressure-Velocity Coupling Options (p. )) for solving the coupled

system of equations arising in multiphase flows are:

Schemes

Phase Coupled SIMPLE (Eulerian multiphase)

PISO (VOF and mixture)

SIMPLE (VOF and mixture)

SIMPLEC (VOF and mixture)

Coupled (all multiphase models)

Options

Coupled with Volume Fractions (all multiphase models except drift-flux)

Solve N-Phase Volume Fraction Equations (mixture and Eulerian models)

The PISO, SIMPLE, and SIMPLEC schemes apply to the VOF and mixture models and are discussed in

Pressure-Velocity Coupling in the Theory Guide.

The Phase Coupled SIMPLE (PC-SIMPLE) is an extension of the SIMPLE algorithm  [] (p. ) to

multiphase flows. The velocities are solved coupled by phases in a segregated fashion. Fluxes are re-

constructed at the faces of the control volume and then a pressure correction equation is built based

on total continuity. The coefficients of the pressure correction equations come from the coupled per

phase momentum equations. This method has proven to be robust and it is the only method available

for all previous versions of ANSYS Fluent.

The Coupled scheme (also known as Multiphase Coupled in previous ANSYS Fluent versions) solves

all equations for phase velocity corrections and shared pressure correction simultaneously  [] (p. ).

These methods incorporate the lift forces and the mass transfer terms implicitly into the general matrix.

This method works very efficiently in steady-state situations, or for transient problems when larger

time steps are required.

The Coupled with Volume Fractions option (also known as Full Multiphase Coupled in previous

ANSYS Fluent versions) couples velocity corrections, shared pressure corrections, and the correction

for volume fraction simultaneously. Theoretically, it should be more efficient, however it may have

some drawbacks in robustness and CPU time usage. The robustness issue stems from the lack of control

of the solution of the volume fraction equation. The continuity constraint (sum of all volume fractions

equals , and individual values limited between zero and one) cannot be enforced exactly during inner

solver iterations, and slight variations from the physical limits may lead to divergence. Research is

ongoing in this area to improve the method. The method is advantageous for heterogeneous mass

transfer when a low Courant number is given; it also works well in dilute situations.

The Volume Fraction Coupling Method aims to achieve a faster steady-state solution compared to the

segregated method of solving equations. It may not be a suitable option for transient applications due

to the significant overhead in CPU time compared to the segregated method, unless it is run with a

larger time step size.

Note

The Coupled with Volume Fractions option is available in the interface after you have

selected Coupled from the Scheme drop-down list for Pressure-Velocity Coupling.

For steady-state cases, the Pseudo Transient option will be enabled automatically

when you enable the Coupled with Volume Fractions option for the VOF and mixture

models.

models.

Figure . : The Solution Methods Task Page Displaying The Pressure-Velocity Coupling Options

.... Limitations and Recommendations of the Coupled with Volume Fraction

Options for the VOF and Mixture Models

The coupled with volume fractions option has the following limitations:

It is not available when Slip Velocity is enabled for the Mixture multiphase model.

It is not supported when using the Singhal-Et-Al cavitation model.

It is not supported when the Explicit formulation for volume fraction is selected.

Recommended uses of the coupled with volume fractions option:

The Pseudo-transient solver is recommended for steady-state calculations.

It is recommended that you use lower under-relaxation factors for momentum for higher order

schemes.

For marine applications, it is recommended that you use a low-order variant or hybrid treatment for

the Rhie-chow face flux interpolation (see High-Order Rhie-Chow Face Flux Interpolation (p. )).

It is recommended that you use the expert text command options solve/set/coupled-vof-

expert for better stability when using the VOF model (see solve/ in the Text Command List).

.... Solving N-Phase Volume Fraction Equations

For a multiphase flow, the sum of the phase volume fractions must always equal . By default, Fluent

enforces this constraint by solving the volume fraction equations for each of the secondary phases

and then setting the volume fraction of the primary phase to the complement.

In certain cases, where poor convergence and/or mass imbalance are observed, enabling Solve N-

Phase Volume Fraction Equations may improve solutions, although in practice the results obtained

from using this option are case dependent. If selected, this option will solve all volume fraction

equations, including both primary and secondary phases. The resulting phase volume fractions are

then scaled in order to satisfy the requirement of summing to . This approach is more computationally

expensive than the default approach and, in general, should not be necessary for the simulation.

Note

The Solve N-Phase Volume Fraction Equations option is not available for the Volume

of Fluid model or Eulerian with Multi-Fluid VOF Model enabled.

When using the Coupled with Volume Fractions scheme, you will need to specify the following in

the Solution Controls task page (see Figure . : The Solution Controls Task Page Displaying the

Coupled Volume Fraction Method for the VOF and Mixture Models (p. )):

VOF and Mixture Multiphase Model:

– For steady-state cases using the pseudo transient solver, specify the Volume Fraction Courant

Number, and the Pseudo Transient Explicit Relaxation Factors.The Pseudo Transient Explicit

Relaxation Factors are described in Setting Pseudo Transient Explicit Relaxation Factors (p. ).

Note

The Pseudo Transient Explicit Relaxation Factors for the Volume Fraction is

set to . by default.

– For transient cases or steady-state cases not involving the pseudo transient solver, enter the Flow

Courant Number, the Volume Fraction Courant Number, Explicit Relaxation Factors, and the

Under-Relaxation Factors.

Note

The Volume Fraction is set as an Explicit Relaxation Factor and is . by default.

Figure . : The Solution Controls Task Page Displaying the Coupled Volume Fraction

Method for the VOF and Mixture Models

Eulerian Multiphase Model:

For steady-state cases using the pseudo transient solver, specify the Pseudo Transient Explicit

Relaxation Factors as described in Setting Pseudo Transient Explicit Relaxation Factors (p. ).

Note

–

Courant Number, the Explicit Relaxation Factors, and the Under-Relaxation Factors.

Note

The under-relaxation for Volume Fraction is set by using an implicit Under-Relax-

ation Factor, rather than a Volume Fraction Courant Number, and is . by de-

fault.

Method for the Eulerian Multiphase Model

Several recommendations for improving the accuracy and convergence of the VOF solution are

presented here.

.... Setting the Reference Pressure Location

The site of the reference pressure can be moved to a location that will result in less round-off in the

pressure calculation. By default, the reference pressure location is the center of the cell at or closest

to the point (,,). You can move this location by specifying a new Reference Pressure Location

in the Operating Conditions Dialog Box (p. ).

Setup →

The position that you choose should be in a region that will always contain the least dense of the

fluids (for example, the gas phase, if you have a gas phase and one or more liquid phases). This is

because variations in the static pressure are larger in a more dense fluid than in a less dense fluid,

given the same velocity distribution. If the zero of the relative pressure field is in a region where the

pressure variations are small, less round-off will occur than if the variations occur in a field of large

nonzero values. Thus in systems containing air and water, for example, it is important that the reference

pressure location be in the portion of the domain filled with air rather than that filled with water.

.... Pressure Interpolation Scheme

For all VOF calculations, you should use the body-force-weighted pressure interpolation scheme or

the PRESTO! scheme.

Solution →

Controls

.... Discretization Scheme Selection

The availability of discretization schemes for volume fraction is summarized in Spatial Discretization

Schemes for Volume Fraction (p. ).

If you are modeling a sharp interface regime on meshes that have high aspect ratio cells, large jumps

in cell size, or high skewness, interface capturing schemes such as Compressive and CICSAM will

not produce very sharp results. For such cases, you should use the Geo-Reconstruct scheme.

For meshes of good quality, it is recommended that you use the Compressive scheme, which is

available in both explicit and implicit formulations and is applicable to both sharp and dispersed flow

regimes. The Compressive scheme also provides better accuracy compared with CICSAM and Mod-

ified HRIC for most cases. When used with the implicit formulation and the second order time scheme,

the Compressive scheme produces quite a sharp interface.

When using the Compressive spatial discretization scheme, it is recommended that you use step-

wise sharpening after the flow transitions from the diffused zone to the sharpening zone. In other

words, you would want to transition from first order to second order, followed by a transition from

second order to compressive. You would want to take this approach if the flow has a smooth transition

from a sharp interfacial zone to a diffused interfacial zone. However, if the flow has a nonuniform

transition from a diffused interfacial zone to a sharp interfacial zone, this might create unphysical

sharpening of the interface if not handled properly, especially for transient cases. For example,

transitioning from a slope limiter of  (compressive) to a slope limiter of  or  (first order or second

order) might be acceptable, but a first order to compressive transition might create unphysical

sharpening of the interface.

If you are solving a problem with the evaporation-condensation mass transfer mechanism enabled

(Including Mass Transfer Effects (p. )) it is recommended that you use one of the diffusive interface

capturing schemes such as QUICK, HRIC, or Phase Localized Compressive (Discretizing Using the

Phase Localized Compressive Scheme (p. )).

Important

The BGM scheme produces a sharp interface, which may result in poor convergence in

some cases. In such situations, we recommend you use a low value for the VOF under-re-

laxation. In addition, you can start with the Compressive or Modified HRIC scheme and

then switch to the BGM scheme.

.... High-Order Rhie-Chow Face Flux Interpolation

In VOF modeling, using a high-order discretization scheme for the momentum transport equations

may reduce the stability of the solution compared to cases using first-order discretization. In such

situations, there are a couple of recommendations:

. Use a low-order variant of the Rhie-Chow face flux interpolation.This is enabled using the following

solve → set → numerics

You will be asked

disable high order Rhie-Chow flux? [no]

to which you will respond yes.

. Use a hybrid treatment of high-order Rhie-Chow face flux interpolation.This is enabled using the

solve → set → vof-numerics

Use hybrid treatment for high order Rhie-Chow flux? [no]

Hybrid treatment allows you to use a high-order variant of the Rhie-Chow face flux interpol-

ation everywhere inside the domain, except in the vicinity of the interface where a low-order

variant is used for the interpolation of the face flux. This treatment could be helpful to get

better convergence without compromising much of the accuracy.

....Treatment of Unsteady Terms in Rhie-Chow Face Flux Interpolation

For cases using Moving Mesh/Dynamic Mesh/Multiple Reference Frame models, ANSYS Fluent does

not consider the unsteady terms for Rhie-Chow face flux interpolation by default. Accounting for the

unsteady terms helps to achieve better solution stability, especially when using a lower time step

size with the PRESTO scheme.

To enable forced treatment of unsteady terms in Rhie-Chow face flux interpolation, use the following

Use forced treatment of unsteady terms in Rhie-Chow flux? [no]

.... Using Unstructured Variant of PRESTO Pressure Scheme

For hexahedral and quadrilateral meshes, ANSYS Fluent uses the structured variant of the PRESTO

scheme by default. For certain cases with non-conformal grid interfaces, the structured variant produces

unexpected behavior at the intersection of the fluid-fluid and non-conformal grid interfaces. For these

cases, using an unstructured variant of PRESTO provides better solution stability and avoids unexpec-

tedly high velocities in the vicinity of the non-conformal grid interfaces.

To enable the unstructured variant of the PRESTO scheme, use the following text command:

Use unstructured variant of PRESTO pressure scheme? [no]

Note

Note

The unstructured variant of PRESTO is automatically enabled for cases involving an unstruc-

tured mesh and this option is redundant in its usage.

.... Pressure-Velocity Coupling and Under-Relaxation for the Time-dependent

Another change that you should make to the solver settings is in the pressure-velocity coupling

scheme and under-relaxation factors that you use. The PISO scheme is recommended for transient

calculations in general. Using PISO allows for increased values on all under-relaxation factors, without

a loss of solution stability. You can generally increase the under-relaxation factors for all variables to

and expect stability and a rapid rate of convergence (in the form of few iterations required per time

step). For calculations on tetrahedral or triangular meshes, an under-relaxation factor of .–. for

pressure is recommended for improved stability with the PISO scheme.

Solution →

Controls

As with any ANSYS Fluent simulation, the under-relaxation factors will need to be decreased if the

solution exhibits unstable, divergent behavior with the under-relaxation factors set to . Reducing

the time step is another way to improve the stability.

.... Under-Relaxation for the Steady-State Formulation

If you are using the steady-state implicit VOF scheme, the under-relaxation factors for all variables

should be set to values between . and . for improved stability.

.... Setting the Under-Relaxation Factor for the Slip Velocity

You should begin the mixture calculation with a low under-relaxation factor for the slip velocity. A

value of . or less is recommended. If the solution shows good convergence behavior, you can increase

this value gradually.

.... Calculating an Initial Solution

For some cases (for example, cyclone separation), you may be able to obtain a solution more quickly

if you compute an initial solution without solving the volume fraction and slip velocity equations.

Once you have set up the mixture model, you can temporarily disable these equations and compute

an initial solution.

Solution →

Controls

In the Equations Dialog Box (p. ), deselect Volume Fraction and Slip Velocity in the Equations

list. You can then compute the initial flow field. Once a converged flow field is obtained, turn the

Volume Fraction and Slip Velocity equations back on again, and compute the mixture solution.

To improve convergence behavior, you may want to compute an initial solution before solving the

complete Eulerian multiphase model. There are multiple methods you can use to obtain an initial

solution for an Eulerian multiphase calculation:

Set up and solve the problem using the mixture model (with slip velocities) instead of the Eulerian model.

You can then enable the Eulerian model, complete the setup, and continue the calculation using the

mixture-model solution as a starting point.

Set up the Eulerian multiphase calculation as usual, but compute the flow for only the primary phase.To

do this, deselect Volume Fraction in the Equations list in the Equations Dialog Box (p. ). Once you

have obtained an initial solution for the primary phase, turn the volume fraction equations back on and

continue the calculation for all phases.

Use the mass-flow inlet boundary condition to initialize the flow conditions. It is recommended that you

set the value of the volume fraction close to the value of the volume fraction at the inlet.

At the beginning of the solution, a lower time step is recommended in order to reach convergence.

If using the volume fraction explicit scheme, do not start with a large Courant number at the beginning

of your run.

If using the volume fraction explicit scheme, start a run with a lower time step and then increase

the time step size. Alternatively, this could be done by using multiphase-specific time stepping,

which would increase the time step size based on the input parameters.

For problems involving a free surface or sharp interfaces between the phases, it is recommended that

you use the symmetric drag law, available in the Phase Interaction Dialog Box (p. ).

Multiphase-specific time stepping is not recommended for compressible flows.

Important

You should not try to use a single-phase solution obtained without the mixture or Eulerian

model as a starting point for an Eulerian multiphase calculation. Doing so will not improve

convergence, and may make it even more difficult for the flow to converge.

....Temporarily Ignoring Lift and Virtual Mass Forces

If you are planning to include the effects of lift and/or virtual mass forces in a steady-state Eulerian

multiphase simulation, you can often reduce stability problems that sometimes occur in the early

stages of the calculation by temporarily ignoring the action of the lift and the virtual mass forces.

Once the solution without these forces starts to converge, you can interrupt the calculation, define

these forces appropriately, and continue the calculation.

.... Using W-Cycle Multigrid

For problems involving a packed-bed granular phase with very small particle sizes (on the order of

m), convergence can be obtained by using the W-cycle multigrid for the pressure. In the Multigrid

tab, under Fixed Cycle Parameters in the Advanced Solution Controls Dialog Box (p. ), you may

need to use higher values for Pre-Sweeps, Post-Sweeps, and Max Cycles. When you are choosing

the values for these parameters, you should also increase the Verbosity to  in order to monitor the

AMG performance; that is, to make sure that the pressure equation is solved to a desired level of

convergence within the AMG solver during each global iteration. See Defining the Phases for the

Eulerian Model (p. ) for more information about granular phases, and The V and W Cycles in the

Theory Guide and Modifying Algebraic Multigrid Parameters (p. ) for details about multigrid cycles.

.... Including the Anisotropic Drag Law

When using the anisotropic drag law (Including the Multi-Fluid VOF Model (p. )), it is recommended

that you start the solution with a lower anisotropy ratio. After your solution has run for some time,

you can then increase the ratio by reducing the friction factor in the tangential direction. Note that

You can also start the solution with the symmetric drag law, then change to the anisotropic drag law.

Using a smaller under-relaxation for pressure and momentum may also help in convergence for cases

with a higher anisotropy ratio.

If the flow for a particular phase is important in both directions (normal and tangential to the interface),

use a lower anisotropy ratio, between -. A higher anisotropy ratio might cause an unstable

solution for such cases. For a higher anisotropy ratio of more than , a smaller under-relaxation

for pressure and momentum is recommended. When using the coupled multiphase solver, if the

solution is unstable with a higher anisotropy ratio, then reducing the courant number may be bene-

ficial. Anisotropic Drag Method [], with Viscosity option [] is recommended for a

higher viscosity ratio.

.... Controlling NITA Solution Options via the Text Interface

For the Eulerian multiphase model, the Non-Iterative Time Advancement (NITA) scheme uses PISO as

a pressure velocity coupling method, where the pressure correction equation is solved in two steps

named predictor and corrector.

For the face pressure calculation, the Eulerian multiphase model uses PRESTO as a default method

for both the predictor and corrector steps.

You can change the face pressure interpolation method using the following text command:

solve/set/multiphase-numerics/nita-controls/face-pressure-options

To select Body Force Weighted as a face pressure interpolation method for both predictor and cor-

rector steps, enter yes  at the enable body-force-weighted for face pressure

calculation? prompt.

To select the Second Order method as a face pressure interpolation method for both predictor and

corrector steps:

. Enter no  at the enable body-force-weighted for face pressure calculation?

prompt.

. When prompted with face pressure calculation method for predictor step, choose

Second Order (  ).

To select the Second Order method as a face pressure interpolation method for the corrector step

only:

prompt.

. When prompted with face pressure calculation method for predictor step, retain

the default selection of PRESTO (  ).

. When prompted with face pressure calculation method for corrector step, choose

Second Order (  ) .

When PRESTO is used for the face pressure calculation, you will be asked whether you want to exclude

transient terms. Because the impact of fluxes on the face pressure is inversely proportional to the

time step size, which may lead to numerical problems as the time step size decreases, the exclusion

of transient terms is recommended for very small time steps when using PRESTO:

exclude transient terms in face pressure calculation? [no] yes

.... Boundary Conditions, Initialization, and Patching

When you use the wet steam model (described in Wet Steam Model Theory in the Theory Guide, and

Setting Up the Wet Steam Model (p. )), the following two field variables will show up in the inflow,

outflow boundary dialog boxes, and in the Solution Initialization task page and Patch dialog boxes.

Liquid Mass Fraction (or the wetness factor)

In general, for dry steam entering flow boundaries the wetness factor is zero.

Log10 (Droplets Per Unit Volume)

In general this value is set to zero, indicating zero droplets entering the domain.

.... Solution Limits for the Wet Steam Model

When you select the wet steam model for the first time, a message is displayed indicating that the

Minimum Static Temperature should be adjusted to  K since the accuracy of the built-in steam

data is not guaranteed below a value of  K. If you use your own steam property functions, you

can adjust this limit to whatever is permissible for your data.

To adjust the temperature limits, go to the Solution Limits dialog box.

Limits...

The default maximum wetness factor or liquid mass fraction ( ) is set to .. In general, during the

convergence process, it is common that this limit will be reached, but eventually the wetness factor

will drop below the value of .. However, in cases where the limit must be adjusted, you can do so

using the text user interface.

define → models → multiphase → wet-steam → set → max-liquid-mass-fraction

Important

Note that the maximum wetness factor should not be set beyond . since the present

model assumes a low wetness factor. When the wetness factor is greater than ., the

solution tends to be less stable due to the large source terms in the transport equations.

Thus, the maximum wetness factor has been set to a default value of ., which corresponds

to the fact that most nozzle and turbine flows will have a wetness factor less than ..

.... Solution Strategies for the Wet Steam Model

If you face convergence difficulties while solving wet steam flow, try to initially lower the CFL value

and use first-order discretization schemes for the solution. If you are still unable to obtain a converged

solution, then try the following solver settings:

. Lower the under-relaxation factor for the wet steam equation below the current set value.The under-

relaxation factor can be found in the Solution Controls task page.

Solution →

Controls

. Solve for an initial solution with no condensation. Once you have obtained a proper initial solution, turn

on the condensation.

To turn condensation on or off, go to the Solution Controls task page.

Solution →

Controls

In the Equations dialog box, deselect Wet Steam in the Equations list. When doing so, you are

preventing condensation from taking place while still computing the flow based on steam prop-

erties. Once a converged flow field is obtained, turn the Wet Steam equation back on again and

compute the mixture solution.

.. Multiphase Case Check

You can check the multiphase case setup using the multiphase check function available via the text

user interface (TUI) command:

/report/mphase-summary

This function prints for you a summary of useful settings, important model information, and recommend-

ations for choosing case parameters. Your case will be checked for compliance in the following categories:

MODELING

MESHING

PHASES

PHASE INTERACTION

BOUNDARY CONDITIONS

CELL ZONE CONDITIONS

OPERATING CONDITIONS

SOLVER METHODS/CONTROLS

ADVANCED SOLVER NUMERICS

MULTIPHASE NUMERICS

SOLUTION LIMITS

MONITORS/RESIDUALS

INITIALIZATION

RUN CALCULATION

POST PROCESSING

Important

Important

To execute this command, a case and valid data (solution or initialization) are required. If

the case has been modified, you need to either reinitialize or rerun the case.

When prompted for verbosity, you can set the level of detail for the report. A value of  (the default)

corresponds to a basic report, while a value of  corresponds to a more detailed report.

In each category, established rules and built-in best practices will be available, along with recommended

changes to your current settings. At your discretion, you may choose to apply the recommendations,

or keep your current settings. Refer to the appropriate sections in the Fluent User's Guide (p. ) for

more information about the recommended changes.

For VOF cases, you can generate a summary report for the case setup using the VOF Check button that

appears in the Solution Initialization task page after you initialize your case. The action of this button

is similar to the report/mphase-summary text command with the verbosity set to .

.. Postprocessing for Multiphase Modeling

Each of the three general multiphase models provides a number of additional field functions that you

can plot or report. You can also report flow rates for individual phases for all three models, and display

velocity vectors for the individual phases in a mixture or Eulerian calculation.

Information about these postprocessing topics is provided in the following subsections:

... Model-Specific Variables

... Displaying Velocity Vectors

... Reporting Fluxes

... Reporting Forces on Walls

... Reporting Flow Rates

When you use one of the general multiphase models, some additional field functions will be available

for postprocessing, as listed in this section. Most field functions that are available in single phase cal-

culations will be available for either the mixture or each individual phase, as appropriate for the gen-

eral multiphase model and specific options that you are using. See Field Function Definitions (p. )

for a complete list of field functions and their definitions. Displaying Graphics (p. ) and Reporting

Alphanumeric Data (p. ) explain how to generate graphics displays and reports of data.

....VOF Model

For VOF calculations you can generate graphical plots or alphanumeric reports of the following addi-

tional item:

Volume fraction (in the Phases... category)

This item is available for each phase.

The variables that are not phase specific are available (for example, variables in the Pressure... and

Velocity... categories) and represent mixture quantities. Thermal quantities will be available only for

calculations that include the energy equation.

.... Mixture Model

For calculations with the mixture model, you can generate graphical plots or alphanumeric reports

of the following additional items:

Diameter (in the Properties... category)

This item is available only for secondary phases.

Interfacial Area Concentration (in the Interfacial Area Concentration... category)

The variables that are not phase specific are available (for example, variables in the Pressure... category)

represent mixture quantities. Thermal quantities will be available only for calculations that include

the energy equation.

.... Eulerian Model

For Eulerian multiphase calculations you can generate graphical plots or alphanumeric reports of the

following additional items:

Postprocessing for Multiphase Modeling

Granular Conductivity (in the Properties... category)

This item is available only for granular phases.

Granular Pressure (in the Granular Pressure... category)

Granular Temperature (in the Granular Temperature... category)

The availability of turbulence quantities will depend on which multiphase turbulence model you used

in the calculation. Thermal quantities will be available (on a per-phase basis) only for calculations that

include the energy equation.

More advanced options for the mixture phase are available under the Phases... category, allowing

you to select from a list of variables to postprocess. To access the entire list in the graphical user in-

terface, type the following text command:

solve → set → expert

Retain most of the default settings, except when asked to Keep temporary solver memory

from being freed?. Answering yes to this question will expose a list under the Phases category

for the mixture phase, one of which will be the Phase ID. Selecting this option allows you to plot

contours of phase IDs for the volume fraction, which will facilitate phase distribution display when

more than two phases are present for free surface calculations.

Note

The expert option for not freeing temporary solver memory is incompatible with dynamic

adaption in serial and parallel for all multiphase models.

Important

This option is available for all the multiphase models. However, note that only cell values

should be plotted for this option. Make sure that the Node Values option is not selected

as it will show the wrong phase ID contours at the interface.

.... Multiphase Species Transport

For calculations using species transport with either of the multiphase models, you can generate

graphical plots or alphanumeric reports of the following additional items:

Mass Fraction of species-n (in the Species... category)

This item is available for each species.

Mole Fraction of species-n (in the Species... category)

Molar Concentration of species-n (in the Species... category)

Lam. Diff Coeff of species-n (in the Species... category)

Eff. Diff. Coeff. of species-n (in the Species... category)

Enthalpy of species-n (in the Species... category)

Relative Humidity (in the Species... category).

Turbulent Rate of Reaction-n (in the Reactions... category)

Rate of Reaction (in the Reactions... category).

Mass Transfer Rate n (in the Phase Interaction... category)

This item is available for each mass transfer mechanism that you defined.

Thermal quantities will be available only for calculations that include the energy equation.

....Wet Steam Model

ANSYS Fluent provides a wide range of postprocessing information related to the wet steam model.

The wet steam related items can be found in Wet Steam.... category of the variable selection drop-

down list that appears in the postprocessing dialog boxes.

Log10 (Droplets Nucleation Rate)

.... Dense Discrete Phase Model

For postprocessing, both the DPM and the Eulerian multiphase capabilities are retained. In addition

to usual DPM postprocessing (Postprocessing for the Discrete Phase (p. )), you can display, for ex-

ample, vector plots of the particle’s velocity field. Make sure to select the discrete phase from the

Phase drop-down list. For transient simulations that include the dense discrete phase model, you

can display the following when the Unsteady Statistics... category is selected:

Mean Velocity

Mean Volume Fraction

RMSE Velocity

RMSE Volume Fraction

Important

For the Unsteady Statistics... category to appear in the postprocessing dialog boxes, make

sure that Data Sampling for Time Statistics is enabled in the Run Calculation task page,

and that you have performed the calculation.

For mixture and Eulerian calculations, it is possible to display velocity vectors for the individual phases

using the Vectors dialog box.

Results → Graphics → Vectors

Edit...

To display the velocity of a particular phase, select Velocity in the Vectors of drop-down list, and then

select the desired phase in the Phase drop-down list. You can also choose Relative Velocity to display

the phase velocity relative to a moving reference frame. To display the mixture velocity

(relevant

for mixture model calculations only), select Velocity (or Relative Velocity for the mixture velocity re-

lative to a moving reference frame), and mixture as the Phase. Note that you can color vectors by

values of any available variable, for any phase you defined. To do so, make the appropriate selections

in the Color by and following Phase drop-down lists.

When you use the Flux Reports dialog box to compute fluxes through boundaries, you will be able

to specify whether the report is for the mixture or for an individual phase.

Edit...

Edit...

Select mixture in the Phase drop-down list at the bottom of the dialog box to report fluxes for the

mixture, or select the name of a phase to report fluxes just for that phase.

When mass transfer is included in multiphase simulations, ANSYS Fluent by default uses the following

sensible enthalpy definition for the reporting of the enthalpies and total heat transfer rate:

where

is the phase temperature for the Eulerian multiphase model or the mixture temperature for

all other multiphase models,

is the reference temperature,

is the formation enthalpy at

, and

is the specific heat. The values for

,

, and

are those you specified in the

The mixture enthalpy is calculated as a mass-weighted average of the phase enthalpies.

Note

When the Boiling model is used as a mass transfer mechanism, the ANSYS Fluent postprocessing

tools may report the heat transfer rate imbalance that is equal to boiling heat flux (in the absence

of any external heat source).This is not an indicator of any problem because the reported im-

balance is due to explicit handling of boiling heat fluxes.

When using the alternative formulation for modeling energy sources due to mass transfer, you

can refer to Alternative Modeling of Energy Sources (p. ) for heat flux reporting options and

sensible enthalpy definition.

For Eulerian calculations, when you use the Force Reports dialog box to compute forces or moments

on wall boundaries, you will be able to specify the individual phase for which you want to compute

the forces.

Edit...

Edit...

Select the name of the desired phase in the Phase drop-down list on the left side of the dialog box.

You can obtain a report of mass flow rate for each phase (and the mixture) through each flow

boundary using the report/fluxes/mass-flow text command:

report → fluxes → mass-flow

When you specify the phase of interest (the mixture or an individual phase), ANSYS Fluent will give

you the option to list each zone, followed by a summary of the mass flow rate through that zone for

the specified phase, or will summarize the mass flow rate for all zones. An example is shown below,

demonstrating how to list the mass flow rate for all zones.

/report/fluxes> mf

(mixture water air)

domain id/name [mixture] air

all boundary/interior zones [yes]

Write to File? [no]

air

Mass Flow Rate               (kg/s)

-------------------------------- --------------------

spiral-press-outlet           -.

pressure-outlet           -.

spiral-vel-inlet            .

walls

velocity-inlet            .

---------------- --------------------

Net           -.

Note

The mass flow rate is calculated through the simulation domain or the specified zones.

However, if you specify only the interior zone(s), the net mass flow rate may show as ,

because these internal boundaries are skipped when ANSYS Fluent computes the net influx

and outflux.

Chapter : Population Balance Model

This chapter provides basic instructions to install the population balance model and solve population

balance problems in ANSYS Fluent. It assumes that you are already familiar with standard ANSYS Fluent

features, including the user-defined function procedures described in the Fluent Customization Manual.

This chapter describes the following:

.. Population Balance Module Installation

.. Loading the Population Balance Module

.. Population Balance Model Setup

.. Postprocessing for the Population Balance Model

.. UDFs for Population Balance Modeling

.. DEFINE_HET_RXN_RATE Macro

The population balance module is provided as an add-on module with the standard ANSYS Fluent licensed

software.

The population balance module is loaded into ANSYS Fluent through the text user interface (TUI). The

module can only be loaded when a valid ANSYS Fluent case file has been set or read. The text command

to load the module is:

A list of ANSYS Fluent add-on modules is displayed:

> /define/models/addon-module

. None

. MHD Model

Select the Population Balance Model by entering the module number . During the loading

process a Scheme library containing the graphical and text user interface, and a UDF library containing

a set of user defined functions are loaded into ANSYS Fluent. A message Addon Module: pop-

bal...loaded! is displayed at the end of the loading process.

The population balance module setup is saved with the ANSYS Fluent case file. The module is loaded

automatically when the case file is subsequently read into ANSYS Fluent. Note that in the saved case

file, the population balance module is saved with the absolute path. Therefore, if the locations of the

population balance module installation or the saved case file are changed, ANSYS Fluent will not be

able to load the module when the case file is subsequently read.

Following the loading of the population balance module, enable either the mixture or Eulerian multiphase

model. This will enable you to activate the population balance model, where you will specify the appro-

priate parameters, and supply multiphase boundary conditions. These inputs are described in this section.

Using the double-precision version of ANSYS Fluent when solving population balance problems is highly

Important

A limitation of the population balance model is that it can be used only on one secondary

phase, even if your problem includes additional secondary phases. Note that a three-phase

gas-liquid-solid case can be modeled, where the population balance model is used for the

gas phase and the solid phase acts as a catalyst. However, if you are using the Inhomogen-

eous Discrete, more than one secondary phase can be used. Note that the properties of the

secondary phases selected for that method should be the same for consistency.

... Enabling the Population Balance Model

... Defining Population Balance Boundary Conditions

... Specifying Population Balance Solution Controls

... Coupling With Fluid Dynamics

... Specifying Interphase Mass Transfer Due to Nucleation and Growth

The procedure for setting up a population balance problem is described below. (Note that this procedure

includes only those steps necessary for the population balance model itself; you will need to set up

other models, boundary conditions, and so on, as usual. See the ANSYS Fluent User's Guide (p. ) for

details.)

. Start the double-precision version of ANSYS Fluent.

. To enable the population balance model, follow the instructions in Loading the Population Balance

Module (p. ).

Remember to enable the mixture or Eulerian multiphase model.

. Open the Population Balance Model dialog box (Figure . :The Population Balance Model Dialog

Box (p. )).

Setup → Models → Population Balance

Edit...

Population Balance Model

Figure . : The Population Balance Model Dialog Box

. Specify the population balance method under Method.

If you select Discrete, you will need to specify the following parameters:

Population Balance Model Setup

Kv

specifies the value for the particle volume coefficient

(as described in Particle Growth). By default,

this coefficient has a value of

.

Definition

can be specified as a Geometric Ratio or as a File. If Geometric Ratio is selected, then the Ratio

Exponent must be specified. If File is selected, you will click the Load File... button and select the

bin size file that you want loaded.

You can input the diameter through the text file, with each diameter listed on a separate

line, starting from the smallest to the largest diameter (one entry per line). Hence, you are

not limited by the choices specified in the dialog box.

Bins

specifies the number of particle size bins used in the calculation.

Ratio Exponent

specifies the exponent  used in the discretization of the growth term volume coordinate (see Nu-

merical Method).

Min Diameter

specifies the minimum bin size

.

Max Diameter

displays the maximum bin size, which is calculated internally.

To display a list of the bin sizes in the console window, click Print Bins. The bin sizes will be

listed in order of size, from the largest to the smallest. This option is only available when the

Geometric Ratio Definition is selected.

If you select Inhomogeneous Discrete under Method, you will specify the same parameters as for the

Discrete model. Additionally, you can include more than one secondary phase in the bin definition.

Enter the total number of Active Secondary Phases in your simulation.

Note

While reading bins through the Load File... option for the Inhomogeneous Discrete

model, the corresponding phase name must be included, for example (("air-"

(. . .))

If you select Standard Moment under Method, you will specify the number of Moments under Para-

meters.

If you selected Quadrature Moment under Method, you will set the number of moments to either ,

or  under Parameters.

If you selected DQMOM under Method, you will select the DQMOM Phases from the list.You will also

specify the following Parameters:

Max Size

specifies the maximum size of the particle.

Min Size

specifies the minimum size of the particle.

Max Size

Min Size

Reference Length

is the reference particle size. Normally, the averaged size of the particle group should be sufficient.

Min VOF

is the minimum VOF, where the total volume fraction of the particle phases (participating in DQMOM

computations) is below the minimum value; the source terms caused by the breakage and coales-

cence are not computed in that cell for the DQMOM and VOF equations.

Max VOF Change/Time Step

is the maximum VOF change in percentage for each DQMOM phase per time step, in order to

smooth the convergence progress.

Generate DQMOM Values

enables you to generate DQMOM values from PDF, CDF, or Overall Moments files. Each of the file

formats and the way to generate the values are discussed in Generated DQMOM Values (p. ).

Note

The DQMOM method is restricted to a four-phase system, of which three secondary

phases are directly involved in the DQMOM computation. Unsteady simulations are

required to model breakage and coalescence and a well defined initial field is recom-

mended, in which the abscissas are distinct. Only growth, breakage, and aggregation

are the available phenomena. No nucleation is considered.

. Select the secondary phase from the Phase drop-down list for which you want to apply the population

balance model parameters.

. For all population balance methods, you can enable the following under Phenomena :

enables you to specify the nucleation rate (

).You can select constant or user-defined

from the drop-down list. If you select constant, specify a value in the adjacent field. If you have a user-

defined function (UDF) that you want to use to model the nucleation rate, you can choose the user-

defined option and specify the appropriate UDF.

Note

This option is not available when using the Inhomogeneous Discrete method.

Growth Rate

enables you to specify the particle growth rate (m/s).You can select constant or user-defined from

the drop-down list. If you select constant, specify a value in the adjacent field. If you have a user-

defined function (UDF) that you want to use to model the growth rate, you can choose the user-

Note

Aggregation Kernel

enables you to specify the aggregation kernel (

) and specify the Aggregation Factor.

The Aggregation Factor (

in Equation . in the Fluent Theory Guide) is used for the calib-

ration of the aggregation kernel.

For Rate, you can select constant, luo-model, free-molecular-model, turbulent-model, prince-

blanch-model, or user-defined from the drop-down list:

If you select constant, specify a value in the adjacent field.

If you select luo-model, the Surface Tension for Population Balance dialog box will open auto-

matically to enable you to specify the surface tension (see Figure . :The Surface Tension for

Population Balance Dialog Box (p. )).The aggregation rate for the model will then be calculated

based on Luo’s aggregation kernel (as described in Particle Birth and Death Due to Breakage and

Aggregation).

Figure . : The Surface Tension for Population Balance Dialog Box

If you select free-molecular-model, then Equation . is applied.

If you select turbulent-model, the Hamaker Constant for Population Balance dialog box will

open automatically to enable you to specify the Hamaker constant (see Figure . :The Hamaker

Constant for Population Balance Dialog Box (p. )). More information about this model is available

in Turbulent Aggregation Kernel.

Figure . : The Hamaker Constant for Population Balance Dialog Box

If you select prince-blanch-model, the Prince and Blanch Model Parameters dialog box will open

automatically. Note that because this is a modal dialog box, you must tend to it immediately.

Figure . : The Prince and Blanch Model Parameters Dialog Box

You can specify the following parameters:

– Surface Tension

– Initial Film Thickness: Is

– Final Film Thickness: Is

– Buoyancy Coalescence Coefficient: Is

– Turbulence Coalescence Coefficient: Is

More information about this model is available in Prince and Blanch Aggregation Kernel.

If you have a user-defined function (UDF) that you want to use to model the aggregation rate, you

can choose the user-defined option and specify the appropriate UDF.

Breakage Kernel

enables you to specify the particle breakage frequency (

) and the Breakage Factor.

The Breakage Factor (

in Equation . in the Fluent Theory Guide) is used for the calibration

of the breakage kernel.

For Frequency, you can select constant, luo-model, lehr-model, ghadiri-model, laakkonen-

model or user-defined from the Frequency drop-down list:

Population Balance Dialog Box (p. )).The frequency used in the breakage rate will then be calcu-

lated based on Luo’s breakage kernel (as described in Particle Birth and Death Due to Breakage and

If you select lehr-model, the Surface Tension and Weber Number dialog box will open automat-

ically to enable you to specify the surface tension and critical Weber number (see Figure . :The

Surface Tension and Weber Number Dialog Box (p. )).The frequency used in the breakage rate

will then be calculated based on Lehr’s breakage kernel (as described in Particle Birth and Death

Due to Breakage and Aggregation).

Figure . : The Surface Tension and Weber Number Dialog Box

If you select ghadiri-model, the Ghadiri Breakage Constant for Population Balance dialog box

will open automatically to enable you to specify the breakage constant (see Figure . :The Ghadiri

Breakage Constant for Population Balance Dialog Box (p. )).The frequency will then be calculated

based on Ghadiri’s breakage kernel (as described in Particle Birth and Death Due to Breakage and

Figure . : The Ghadiri Breakage Constant for Population Balance Dialog Box

If you select laakkonen-model, the Surface Tension for Population Balance dialog box will open

automatically to enable you to specify the Surface Tension and the constant C2 (Laakkonen

Breakage Kernels).The frequency will then be calculated based on Laakkonen's breakage kernel (as

described in Laakkonen Breakage Kernels).

If you have a user-defined function (UDF) that you want to use to model the frequency for the

breakage rate, you can choose the user-defined option and specify the appropriate UDF.

If you selected constant, ghadiri-model, laakkonen-model, or user-defined for Frequency,

then you can specify the probability density function used to calculate the breakage rate by

making a selection in the PDF drop-down list. You can select parabolic, laakkonen, generalized,

or user-defined :

If you select parabolic, the Shape Factor for Parabolic PDF dialog box will open automatically to

enable you to specify the shape factor C (see Figure . :The Shape Factor for Parabolic PDF Dialog

Box (p. )).The PDF used in the breakage rate will then be calculated according to Equation .

(as described in Particle Birth and Death Due to Breakage and Aggregation).

Figure . : The Shape Factor for Parabolic PDF Dialog Box

If you select generalized, the Generalized pdf for multiple breakage dialog box will open auto-

matically (Figure . :The Generalized pdf for multiple breakage Dialog Box (p. )).

Figure . : The Generalized pdf for multiple breakage Dialog Box

Perform the following steps in the Generalized pdf for multiple breakage dialog box:

a.

a.

Select either One Term or Two Term from the Options list.Your selection will determine

whether  in Equation . is  or , respectively.

b. Enter a value for the averaged Number of Daughters. It can be any real number (including

non-integers, such as . ), as long as it is not less than .

c.

Define the parameter(s) for Equation . in the Input Parameters group box.When One

Term is selected from the Options list, you must enter a value for qi0.When Two Term is selected

from the Options list, you must enter values for wi0, pi0, qi0, ri0, and qi1. For information

about appropriate values for these parameters to result in the daughter distributions shown in

Table . : Daughter Distributions, see Table . : Daughter Distributions (cont. ).

Note

For the equal-size generalized pdf breakage distribution, the value for qi0

should be set to 1e20.

d. Click the Validate/Apply button to save the settings.The text boxes in the All Parameters

group box will be updated, using the values you entered in the Input Parameters group box,

as well as values derived from the constraints shown in Equation . – Equation ..

e. Verify that the values in the All Parameters group box represent your intended PDF before

clicking Close.

If you have a user-defined function (UDF) that you want to use to model the PDF for the breakage

rate, you can choose the user-defined option and specify the appropriate UDF. See UDFs for Pop-

ulation Balance Modeling (p. ) for details about UDFs for the population balance model.

Choose between the default Hagesather formulation and the Ramakrishna formulation. Detailed

information about these two methods can be found in Breakage Formulations for the Discrete

Method.

. (Discrete and QMOM models only) If you want to account for bubble expansion due to large changes in

hydrostatic pressure in compressible flows, enable Include Expansion.The bubble expansion is modeled

as a growth term in the Population Balance equations (Equation . ).This can be relevant in applications

such as deep-water drilling. For more information, see Particle Growth.

Note

The secondary phase must be modeled as compressible. This option is currently available

for Discrete and QMOM only.

. Specify the boundary conditions for the solution variables.

Setup →

See Defining Population Balance Boundary Conditions (p. ) below.

. Specify the initial guess for the solution variables.

Solution →

. Solve the problem and perform relevant postprocessing functions.

Solution →

See Postprocessing for the Population Balance Model (p. ) for details about postprocessing.

.... Generated DQMOM Values

When using the DQMOM model, you have the option of generating DQMOM values from three dif-

ferent file formats. To do so, select Overall Moments, PDF or CDF under Generate DQMOM Values

and then click the Load File… button. The Select File dialog box will open where you will select the

appropriate file. Clicking OK in the Select File dialog box will result in the file being read and calcu-

lations carried out. The DQMOM values will be printed in the console.

Figure . : The Population Balance Model Dialog Box for the DQMOM Model

DQMOM Values Produced From PDF, CDF Files, or Overall Moments for the Particles

Three quadrature points are assumed, namely QP0, QP1, and QP2 (see Figure . : DQMOM Values

Produced From a PDF File (p. )).

Length, Volume Fraction , and DQMOM-m4 values are given.The latter two can be used for

initial fields of VOF and DQMOM as well as boundary conditions.

For verification purposes, the first six moments are also given together with the total volume fraction

of all particles from the PDF or CDF file. It is your responsibility to make sure that these values are

correct, especially the total volume fraction.

The definition of the first six moments of the particles is length based for the overall moments, de-

scribed in The Quadrature Method of Moments (QMOM).

In PDF or CDF format, the resultant volume fraction is normally given as unity. If you want the real

particle volume fraction to be reflected in the mixture, the second column of the PDF or CDF data

file need to be multiplied by the value of the real volume fraction. Another way is to multiply the

values of the generated DQMOM volume fraction and DQMOM-m4 using the real particle volume

fraction.

Figure . : DQMOM Values Produced From a PDF File

PDF File Format

The probability density function (PDF) is defined by the probability distribution of particles in terms

of the volume fraction over the particle length (namely the diameter of the particle).

The integration of PDF over all possible particle length (normally from  to the maximum diameter)

shall give a value of unity or the real value of the volume fraction of all participating particles.

The following file format is required (as shown below):

– An integer number specified in the first line, indicating the number of data pairs to follow

– The data in the 1st column specifying the length or diameter of particles in ascending order in

meters (m)

– The data in the 2nd column specifying the probability density function. Be aware that the integration

of the PDF over the length shall result in a value of volume fraction for that particular particle

length range

5e- .000058e6

10e- .000271e6

15e- .000669e6

20e- .001264e6

25e- .002062e6

30e- .003055e6

35e- .004228e6

40e- .005549e6

45e- .006972e6

50e- .008439e6

55e- .00988e6

60e- .011217e6

65e- .012366e6

70e- .013253e6

75e- .013811e6

80e- .013996e6

85e- .013789e6

90e- .013199e6

95e- .012268e6

100e- .011062e6

105e- .009668e6

110e- .00818e6

115e- .006694e6

120e- .00529e6

125e- .004033e6

130e- .002962e6

135e- .002093e6

140e- .00142e6

145e- .000925e6

150e- .000576e6

155e- .000344e6

160e- .000196e6

170e- .000055e6

180e- .000012e6

190e- .000002e6

200e- .

210e-  .

CDF File Format

The cumulative density function (CDF) is defined as the integration of PDF over all possible particles

up to the length , resulting in a value of volume fraction for all particles less than length .

The value of the CDF at the maximum particle length/diameter shall be unity, or the real value of the

volume fraction of all particles in the mixture.

meters (m)

– The data in the 2nd column specifying the cumulative density function in terms of the volume

fraction of particles

–

at the maximum particle length

5e-

10e- .109e-

15e- .16e-

20e- .175e-

25e- .208e-

30e- .304e-

35e- .614e-

40e- .5e-

44e-   .e-

45e-   .44e-

50e- .573e-

55e- .19e-

60e- .11e-

65e- .17e-

70e- .007e-

75e- .243e-

80e- .397e-

85e- .453e-

90e- .823e-

95e- .53e-

100e- .073e-

105e- 81e-

110e- .057e-

115e- .187e-

120e- .89e-

125e- .897e-

130e- .437e-

135e- .543e-

140e- .523e-

145e- .173e-

150e- .717e-

155e- .007e-

160e- .363e-

170e- .88e-

180e- .16e-

190e- .327e-

200e- .e-

Overall Moments File Format

The third option is to specify the first six moments for all particles as shown below.

– An integer number specified in the first line, indicating the number of data (moments) to follow.

By default, this shall be

– six moments from moment- to moment- are given in that order.The definition of the first six

moments is based on length as described in The Quadrature Method of Moments (QMOM)

– As a check for moments,

. In the values given below, volume

fraction is assumed to be unity and

is assumed to be

.120556e+

.022475e+

.120556e+

.022475e+

.523370e+

.909857e+

.611191e-

.498663e-

To define boundary conditions specific to the population balance model, use the following procedure:

. In the Boundary Conditions task page, select the secondary phase(s) in the Phase drop-down list and

then open the appropriate boundary condition dialog box (for example, Figure . : Specifying Inlet

Boundary Conditions for the Population Balance Model (p. )).

Setup →

Figure . : Specifying Inlet Boundary Conditions for the Population Balance Model

. In the Multiphase tab, under Boundary Condition, select the type of boundary condition for each bin

(for the discrete method) or moment (for SMM and QMOM) as either Specified Value or Specified Flux.

Note that the boundary condition variables (for example, Bin-) are labeled according to the fol-

lowing:

bin/moment - th bin/moment

where the th bin/moment can range from  (the first bin or moment) to

, where

is the

number of bins/moments that you entered in the Population Balance Model dialog box.

. Under Population Balance Boundary Value, enter a value or a flux as appropriate.

If you selected Specified Value for the selected boundary variable, enter a value in the field adjacent

to the variable name.This value will correspond to the variable

in Equation . (for the discrete

method) or

in Equation . (for SMM or QMOM). If you are using either of the discrete methods

and have selected Specified Value for all bins, you can optionally specify a log-normal distribution and

method) or

have Fluent automatically initialize the bin fractions accordingly to a log-normal distribution (see Initial-

izing Bin Fractions With a Log-Normal Distribution (p. )).

If you selected Specified Flux for the selected boundary variable, enter a value in the field adjacent to

the variable name.This value will be the spatial particle volume flux

.

.... Initializing Bin Fractions With a Log-Normal Distribution

When using one of the discrete methods with Specified Value selected as the boundary condition

for all bins, you can have Fluent populate the bin fractions according to a log-normal distribution

characterized by a mean and standard deviation that you supply. For details of the log-normal distri-

bution, refer to The Log-Normal Distribution.

Important

The log-normal initialization feature is only meaningful and should only be used when

Specified Value is selected for all bins under Boundary Condition.

To use the log-normal distribution, perform the following steps.

.

Enable Log Normal in the Boundary Value group box.

.

Enter values for the Mean and Std Dev of the desired distribution.

.

Click Initialize...

In the Equations dialog box (Figure . : The Equations Dialog Box (p. )), equations for each bin

(for example, phase- Bin) will appear in the Equations list.

The default value under Under-Relaxation Factors (in the Solution Controls task page) for the pop-

ulation balance equations is ., and the default Discretization scheme (in the Solution Methods

task page) is First Order Upwind.

Figure . : The Equations Dialog Box

To couple population balance modeling of the secondary phase(s) with the overall problem fluid dy-

namics, a Sauter mean diameter (

in Equation .) may be used to represent the particle diameter

of the secondary phase. The Sauter mean diameter is defined as the ratio of the third moment to the

second moment for the SMM and QMOM. For the discrete method, it is defined as

(.)

To specify the Sauter mean diameter as the secondary phase particle diameter, open the Secondary

Phase dialog box.

Setup → Models → Multiphase → Phases → phase–id – Secondary Phase

Edit...

In the Secondary Phase dialog box (for example, Figure . : The Secondary Phase Dialog box for

Hydrodynamic Coupling (p. )), select sauter-mean from the Diameter drop-down list under Prop-

erties. Note that a constant diameter or user-defined function may also be used.

Figure . : The Secondary Phase Dialog box for Hydrodynamic Coupling

In applications that involve the creation, dissolution, or growth of particles (such as crystallization),

the total volume fraction equation for the particulate phase will have source terms due to these phe-

nomena. The momentum equation for the particulate phase will also have source terms due to the

added mass. In ANSYS Fluent, the mass source term can be specified using the UDF hook

DEFINE_HET_RXN_RATE, as described in DEFINE_HET_RXN_RATE Macro (p. ), or using the

Phase Interaction dialog box, described below.

As an example, in crystallization, particles are created by means of nucleation (

), and a growth rate

( ) can also be specified. The mass transfer rate of formation (in

) of particles of all sizes is

then

(.)

For the discrete method, the mass transfer rate due to growth can be written as

(.)

If the nucleation rate is included in the total mass transfer, then the mass transfer becomes

(.)

Important

For the discrete method, the sources to the population balance equations must sum to the

total mass transfer rate. To access the sources, you can use the macro C_PB_DISCI_PS

(cell, thread, i).

See UDFs for Population Balance Modeling (p. ) for more information about macros for population

balance variables.

For the SMM, only a size-independent growth rate is available. Hence, the mass transfer rate can be

written as

(.)

For the QMOM, the mass transfer rate can be written as

(.)

For both the SMM and QMOM, mass transfer due to nucleation is negligible, and is not taken into ac-

count.

Important

Note that for crystallization, the primary phase has multiple components; at the very least,

there is a solute and a solvent. To define the multicomponent multiphase system, you will

need to activate Species Transport in the Species Model dialog box for the primary phase

after activating the multiphase model. The rest of the procedure for setting up a species

transport problem is identical to setting up species in single phase. The heterogeneous re-

action is defined as:

When the population balance model is activated, mass transfer between phases for non-reacting species

(such as boiling) and heterogeneous reactions (such as crystallization) can be done automatically, in

lieu of hooking a UDF.

For simple unidirectional mass transfer between primary and secondary phases due to nucleation and

growth phenomena of non-reacting species, configure the following settings:

. Open the Phase Interaction dialog box (Figure . :The Phase Interaction Dialog Box for Non-reacting

Species (p. )).

Setup → Models → Multiphase → Phases → Phase–Interactions

Edit...

. Specify the mass transfer of species between the phases:

Figure . : The Phase Interaction Dialog Box for Non-reacting Species

a.

Under the Mass tab, specify the Number of Mass Transfer Mechanisms involved in your case.

b. For each mechanism, specify the phase of the source material under From Phase and the phase of

the destination material phase under To Phase.

c.

From the Mechanism drop down list, select one of the mechanisms:

none

if you do not want any mass transfer between the phases.

for a fixed, user-specified rate.

if you hooked a UDF describing the mass transfer mechanism.

for an automated method of mass transfer, not involving a UDF.The nucleation and the growth

rates calculated by the population balance kernels are used for mass transfer.

Note

For the Inhomogeneous Discrete population balance model, where there is more

than one secondary phase, you can select population-balance as the mechanism

of mass transfer between the solvent phase (say for crystallization) and each of the

solute phases defined under the Inhomogeneous Discrete population balance

model.

d. Click OK to save the settings.

For heterogeneous reactions, configure the following settings:

. For the primary phase, activate the Species Transport model.

. Open the Phase Interaction dialog box (Figure . :The Phase Interaction Dialog Box for a Heterogeneous

Reaction (p. )).

Edit...

. Under the Reactions tab, specify the stoichiometry for the reactant and the product.

Figure . : The Phase Interaction Dialog Box for a Heterogeneous Reaction

. Select population-balance as the Reaction Rate Function.

. Click OK to save the settings.

Either this method or the use of the UDF, described in DEFINE_HET_RXN_RATE Macro (p. ), will

produce the same results.

For the Inhomogeneous Discrete population balance model involving nucleation and growth, you

can select population-balance as the Reaction Rate Function for each heterogeneous reaction

you have set up. To learn how to set up reactions, go to Specifying Heterogeneous Reactions (p. )

ANSYS Fluent provides postprocessing options for displaying, plotting, and reporting various particle

... Population Balance Solution Variables

... Reporting Derived Population Balance Variables

Solution variables that can be reported for the population balance model are:

Bin-i fraction (discrete method only), where i is N- bins/moments.

Number density of Bin-i fraction (discrete method only)

Diffusion Coef. of Bin-i fraction/Moment-i

Sources of Bin-i fraction/Moment-i

Moment-i (SMM and QMOM only)

Abscissa-i (QMOM method only)

Weight-i (QMOM method only)

Bin-i fraction (

) is the total volume fraction for the

th size bin when using the discrete method.

Number density of Bin-i fraction is the number density (

) in

for the

th size bin.

Moment-i is the

th moment of the distribution when using the standard method of moments or the

quadrature method of moments.

Important

Though the diffusion coefficients of the population variables (for example, Diffusion Coef.

of Bin-i fraction/Moment-i) are available, they are set to zero because the diffusion term

is not present in the population balance equations.

Two options are available in the Results ribbon tab that allow you to report computed moments and

number density on selected surfaces or cell zones of the domain.

.... Computing Moments

.... Displaying a Number Density Function

Postprocessing for the Population Balance Model

You can compute moments for the population balance model using the Population Balance Moments

dialog box (Figure . : The Population Balance Moments Dialog Box (p. )).

Results → Model Specific → Population Balance → Moments...

Figure . : The Population Balance Moments Dialog Box

The steps for computing moments are as follows:

. For the discrete method, specify the Number of Moments. For the SMM and QMOM, the number of

moments is set equal to the number of moments that were solved, and therefore cannot be changed.

. For a surface average, select the surface(s) on which to calculate the moments in the Surfaces list.

. For a volume average, select the volume(s) in which to calculate the moments in the Cell Zones list.

. Click Print to display the moment values in the console window.

. To save the moment calculations to a file, click Write... and enter the appropriate information in the

resulting Select File dialog box.The file extension should be .pb.

You can display the number density function for the population balance model using the Number

Density Function dialog box (Figure . : The Number Density Function Dialog Box (p. )).

Results → Model Specific → Population Balance → Number Density...

Figure . : The Number Density Function Dialog Box

The steps for displaying the number density function are as follows:

. Specify the Report Type as either a Surface Average or a Volume Average.

. Under Plot Type, specify how you would like to display the number density function data.

Histogram

displays a histogram of the discrete number density (

Histogram

).The number of divisions in the histogram

is equal to the number of bins specified in the Population Balance Model dialog box.This option

is available only with the discrete method.

Curve

displays a smooth curve of the number density function.

. (Quadrature Moment method only) Specify Diameter Upper Limit to reconstruct the length or volume-

based number density function based on the moments predicted by QMOM (see Reconstructing the

Particle Size Distribution from Moments in the Fluent Theory Guide for more information).

The moments are calculated by integrating the area under the number density curve. The accuracy

of the calculations is dependent on the integration limit. Typically, this is expressed in terms of

the mean of the distribution and is specified in the Diameter Upper Limit field. The default value

of . means that the maximum diameter value considered is . times the mean of the distribution.

. In the Fields list, select the data to be plotted.

Discrete Number Density

(

) is the number of particles per unit volume of physical space in the

th size bin plotted against

particle diameter size .This option is available only with the discrete method.

Length Number Density Function

(

) is the number of particles per unit volume of physical space per unit particle length plotted

against particle diameter.

Volume Number Density Function

(

) is the number of particles per unit volume of physical space per unit particle volume plotted

against particle volume.

(

. Choose the cell zones on which to plot the number density function data in the Cell Zones list.

. Click Plot... to display the data.

. (optional) Click Print to display the number density function data in the console window.

. Click Write to save the number density function data to a file.The Select File dialog box will open, where

you can specify a name and save a file containing the plot data.The file extension should be .pbd.

This section contains the following sections:

... Population Balance Variables

... Population Balance DEFINE Macros

... Hooking a Population Balance UDF to ANSYS Fluent

The macros listed in Table . : Macros for Population Balance Variables Defined in sg_pb.h  (p. )

can be used to return real variables associated with the population balance model. The variables are

available in both the pressure-based and density-based solvers. The macros are defined in the sg_pb.h

header file, which is included in udf.h.

Table . : Macros for Population Balance Variables Defined in sg_pb.h

Returns

Argument Types

Macro

(

) the total volume fraction for the

th size bin

cell_t c, Thread *t,

int i

C_PB_DISCI

th moment

int i

C_PB_SMMI

th moment, where

int i

C_PB_QMOMI

abscissa

, where

int i

C_PB_QMOMI_L

weight

, where

int i

C_PB_QMOMI_W

net source term to

th size bin

int i

C_PB_DISCI_PS

th moment

int i

C_PB_SMMI_PS

int i

th size bin

int i

th moment

int i

Returns

Macro

th moment

int i

C_PB_QMOMI_PS

This section contains descriptions of DEFINE macros for the population balance model. Definitions

of each DEFINE macro are contained in the udf.h header file.

.... DEFINE_PB_BREAK_UP_RATE_FREQ

.... DEFINE_PB_BREAK_UP_RATE_PDF

.... DEFINE_PB_COALESCENCE_RATE

.... DEFINE_PB_NUCLEATION_RATE

.... DEFINE_PB_GROWTH_RATE

....DEFINE_PB_BREAK_UP_RATE_FREQ

You can use the DEFINE_PB_BREAK_UP_RATE_FREQ macro if you want to define the breakage

frequency using a UDF. The function is executed at the beginning of every time step.

..... Usage

DEFINE_PB_BREAK_UP_RATE_FREQ(name, cell, thread, d_1)

Argument Type

UDF name

char name

Cell index

cell_t cell

Pointer to the secondary phase thread associated with d_1

Thread *thread

Parent particle diameter or length

real d_1

Function returns

real

There are four arguments to DEFINE_PB_BREAK_UP_RATE_FREQ: name, cell, thread, and

d_1. You will supply name, the name of the UDF. cell, thread, and d_1 are variables that are

passed by the ANSYS Fluent solver to your UDF.

Included below is an example of a UDF that defines a breakage frequency (see Particle Birth and

Death Due to Breakage and Aggregation) that is based on the work of Tavlarides , such that

(.)

where

and

are constants,  is the dissipation rate,

is the parent diameter,

tension,

is the volume fraction of the dispersed phase, and

(.)

where

and

tension,

is the density of the primary phase.

/************************************************************************

UDF that computes the particle breakage frequency

*************************************************************************/

UDFs for Population Balance Modeling

#include "sg_pb.h"

#include "sg_mphase.h"

DEFINE_PB_BREAK_UP_RATE_FREQ(break_up_freq_tav, cell, thread, d_1)

{

real epsi, alpha, f1, f2, rho_d;

real C1 = ., C2 = ., sigma = . ;

Thread *tm = THREAD_SUPER_THREAD(thread);/*passed thread is phase*/

epsi = C_D(cell, tm);

alpha = C_VOF(cell, thread);

rho_d = C_R(cell, thread);

f1 = pow(epsi, ./. )/((.+epsi)*pow(d_1, ./. ));

f2 = -(C2*sigma*(.+alpha)*(.+alpha))/(rho_d*pow(epsi,./. )*pow(d_1, ./. ));

return C1*f1*exp(f2);

}

....DEFINE_PB_BREAK_UP_RATE_PDF

You can use the DEFINE_PB_BREAK_UP_RATE_PDF macro if you want to define the breakage PDF

using a UDF. The function is executed at the beginning of every time step.

DEFINE_PB_BREAK_UP_RATE_PDF(name, cell, thread, d_1, thread_2, d_2)

UDF name

char name

Cell index

real d_1

Pointer to the secondary phase thread associated with d_2

Thread *thread_2

Diameter of one of the daughter particles after breakage; the second

daughter particle diameter is calculated by conservation of particle

volume

real d_2

real

There are six arguments to DEFINE_PB_BREAK_UP_RATE_PDF: name, cell, thread, d_1,

volume

real d_2

real

thread_2, and d_2. You will supply name, the name of the UDF. cell, thread, d_1, thread_2,

and d_2 are variables that are passed by the ANSYS Fluent solver to your UDF.

Note

thread and thread_2 are the same for the Discrete, QMOM and SMM models. They

may be the same or different depending on whether d_1 and d_2 belong to the same

phase or different phases for the Inhomogeneous model.

Included below is an example of a UDF that defines a breakage PDF (see Particle Birth and Death

Due to Breakage and Aggregation) that is parabolic, as defined in Equation ..

UDF that computes the particle breakage PDF

DEFINE_PB_BREAK_UP_RATE_PDF(break_up_pdf_par, cell, thread, d_1, thread_2, d_2)

{

real pdf;

real kv = M_PI/. ;

real C = . ;

real f_2, f_3, f_4;

real V_prime = kv*pow(d_1,. );

real V = kv*pow(d_2,. );

f_2 = . *pow(V/V_prime,. );

f_3 = -. *(V/V_prime);

f_4 = . ;

pdf = (C/V_prime) + ((.-C/. )/V_prime)*(f_2 + f_3 + f_4);

return . *pdf;

}

....DEFINE_PB_COALESCENCE_RATE

You can use the DEFINE_PB_COALESCENCE_RATE macro if you want to define your own particle

aggregation kernel. The function is executed at the beginning of every time step.

DEFINE_PB_COALESCENCE_RATE(name, cell, thread, d_1, thread_2, d_2)

UDF name

char name

Cell index

UDF name

char name

Cell index

Diameters of the two colliding particles

real d_1, d_2

real

There are six arguments to DEFINE_PB_COALESCENCE_RATE: name, cell, thread, d_1,

thread_2, and d_2. You will supply name, the name of the UDF. cell, thread, d_1, and d_2

are variables that are passed by the ANSYS Fluent solver to your UDF. Your UDF will need to return

the real value of the aggregation rate.

Note

Included below is an example UDF for a Brownian aggregation kernel. In this example, the aggregation

rate is defined as

where

.

UDF that computes the particle aggregation rate

DEFINE_PB_COALESCENCE_RATE(aggregation_kernel,cell,thread,d_1,thread_2,d_2)

{

real agg_kernel;

real beta_0 = .0e- /* aggregation rate constant */

agg_kernel = beta_0*pow((d_1+d_2),. )/(d_1*d_2);

return agg_kernel;

}

....DEFINE_PB_NUCLEATION_RATE

You can use the DEFINE_PB_NUCLEATION_RATE macro if you want to define your own particle

nucleation rate. The function is executed at the beginning of every time step.

DEFINE_PB_NUCLEATION_RATE(name, cell, thread)

UDF name

char name

Cell index

Pointer to the secondary phase thread

real

There are three arguments to DEFINE_PB_NUCLEATION_RATE: name, cell, and thread. You

will supply name, the name of the UDF. cell and thread are variables that are passed by the

ANSYS Fluent solver to your UDF. Your UDF will need to return the real value of the nucleation

rate.

Potassium chloride can be crystallized from water by cooling. Its solubility decreases linearly with

temperature. Assuming power-law kinetics for the nucleation rate,

where

and

.

UDF that computes the particle nucleation rate

DEFINE_PB_NUCLEATION_RATE(nuc_rate, cell, thread)

{

real J, S;

real Kn = .0e10; /* nucleation rate constant */

real Nn = . ; /* nucleation law power index */

real T,solute_mass_frac,solvent_mass_frac, solute_mol_frac,solubility;

real solute_mol_wt, solvent_mol_wt;

Thread *tc = THREAD_SUPER_THREAD(thread); /*obtain mixture thread */

Thread **pt = THREAD_SUB_THREADS(tc);  /* pointer to sub_threads */

Thread *tp = pt[P_PHASE];     /* primary phase thread */

solute_mol_wt = . ; /* molecular weight of potassium chloride */

solvent_mol_wt = . ; /* molecular weight of water */

solute_mass_frac = C_YI(cell,tp,);

/* mass fraction of solute in primary phase (solvent) */

solvent_mass_frac = . - solute_mass_frac;

solute_mol_frac = (solute_mass_frac/solute_mol_wt)/

((solute_mass_frac/solute_mol_wt)+(solvent_mass_frac/solvent_mol_wt));

T = C_T(cell,tp);  /* Temperature of primary phase in Kelvin */

solubility = . *T-. ;

/* Solubility Law relating equilibrium solute mole fraction to Temperature*/

S = solute_mol_frac/solubility; /* Definition of Supersaturation */

if (S == .)

{

J = . ;

}

else

{

J = Kn*pow((S-),Nn);

}

return J;

}

Important

Note that the solubility and the chemistry could be defined in a separate routine and

simply called from the above function.

....DEFINE_PB_GROWTH_RATE

You can use the DEFINE_PB_GROWTH_RATE macro if you want to define your own particle growth

rate. The function is executed at the beginning of every time step.

DEFINE_PB_GROWTH_RATE(name, cell, thread,d_i)

UDF name

char name

Cell index

Particle diameter or length

real d_i

real

There are four arguments to DEFINE_PB_GROWTH_RATE: name, cell, thread, and d_i. You

will supply name, the name of the UDF. cell, thread, and d_i are variables that are passed by

the ANSYS Fluent solver to your UDF. Your UDF will need to return the real value of the growth

rate.

rate.

temperature. Assuming power-law kinetics for the growth rate,

where

m/s and

.

UDF that computes the particle growth rate

DEFINE_PB_GROWTH_RATE(growth_rate, cell, thread,d_1)

{

/* d_1 can be used if size-dependent growth is needed */

/* When using SMM, only size-independent or linear growth is allowed */

real G, S;

real Kg = .8e-; /* growth constant */

real Ng = . ; /* growth law power index */

if (S == .)

{

G = . ;

}

else

{

G = Kg*pow((S-),Ng);

}

return G;

}

Important

if (S == .)

{

G = . ;

}

else

{

}

return G;

}

Important

After the UDF that you have defined using DEFINE_PB_BREAK_UP_RATE_FREQ, DEFINE_PB_

BREAK_UP_RATE_PDF, DEFINE_PB_COALESCENCE_RATE, DEFINE_PB_NUCLEATION_RATE, or

DEFINE_PB_GROWTH_RATE is interpreted or compiled, the name that you specified in the DEFINE

macro argument (for example, agg_kernel) will become visible and selectable in the appropriate

drop-down list under Phenomena in the Population Balance Model dialog box (Figure . : The

Population Balance Model Dialog Box (p. )).

..DEFINE_HET_RXN_RATE Macro

This section discusses the DEFINE_HET_RXN_RATE macro:

... Description

... Usage

... Example

... Hooking a Heterogeneous Reaction Rate UDF to ANSYS Fluent

You need to use DEFINE_HET_RXN_RATE to specify reaction rates for heterogeneous reactions. A

heterogeneous reaction is one that involves reactants and products from more than one phase. Unlike

DEFINE_VR_RATE, a DEFINE_HET_RXN_RATE UDF can be specified differently for different hetero-

geneous reactions.

During ANSYS Fluent execution, the DEFINE_HET_RXN_RATE UDF for each heterogeneous reaction

that is defined is called in every fluid cell. ANSYS Fluent will use the reaction rate specified by the UDF

to compute production/destruction of the species participating in the reaction, as well as heat and

momentum transfer across phases due to the reaction.

A heterogeneous reaction is typically used to define reactions involving species of different phases.

The bulk phase can participate in the reaction if the phase does not have any species (that is, the

phase has fluid material instead of mixture material). Heterogeneous reactions are defined in the Phase

Interaction dialog box.

... Usage

DEFINE_HET_RXN_RATE (name,c,t,r,mw,yi,rr,rr_t)

UDF name

char name

DEFINE_HET_RXN_RATE Macro

Cell index

cell_t c

Cell thread (mixture level) on which heterogeneous

reaction rate is to be applied

Thread *t

Pointer to data structure that represents the current

heterogeneous reaction (see sg_mphase.h)

Hetero_Reaction *r

Matrix of species molecular weights. mw[i][j] will give

molecular weight of species with ID j in phase with

real mw[MAX_PHASES][MAX_SPE_EQNS]

index i. For phase that has fluid material, the molecular

weight can be accessed as mw[i][].

Matrix of species mass fractions. yi[i][j] will give

real yi[MAX_PHASES][MAX_SPE_EQNS]

index i. For phase that has fluid material, yi[i][]

will be .

Pointer to laminar reaction rate

real *rr

Currently not used. Provided for future use.

real *rr_t

void

There are eight arguments to DEFINE_HET_RXN_RATE: name, c, t, r, mw, yi, rr, and rr_t. You

will supply name, the name of the UDF. c, t, r, mw, yi, rr, and rr_t are variables that are passed

by the ANSYS Fluent solver to your UDF. Your UDF will need to set the values referenced by the real

pointer rr.

The following compiled UDF, named arrh, defines an Arrhenius-type reaction rate. The rate exponents

are assumed to be same as the stoichiometric coefficients.

static const real Arrhenius = .e15;

static const real E_Activation = .e6;

#define SMALL_S .e-

DEFINE_HET_RXN_RATE(arrh,c,t,hr,mw,yi,rr,rr_t)

{

Domain **domain_reactant = hr->domain_reactant;

real *stoich_reactant = hr->stoich_reactant;

int *reactant = hr->reactant;

int i;

int sp_id;

int dindex;

Thread *t_reactant;

real ci;

real T = . ; /* should obtain from cell */

/* instead of compute rr directly, compute log(rr) and then take exp */

rr = ;

for (i=; i < hr->n_reactants; i++)

{

sp_id = reactant[i]; /* species ID to access mw and yi */

if (sp_id == -) sp_id = ; /* if phase does not have species,

mw, etc. will be stored at index  */

dindex = DOMAIN_INDEX(domain_reactant[i]);

/* domain index to access mw & yi */

t_reactant = THREAD_SUB_THREAD(t,dindex);

/* get conc. */

ci = yi[dindex][sp_id]*C_R(c,t_reactant)/mw[dindex][sp_id];

ci = MAX(ci,SMALL_S);

rr += stoich_reactant[i]*log(ci);

}

rr += log(Arrhenius + SMALL_S) -

E_Activation/(UNIVERSAL_GAS_CONSTANT*T);

/* .e- < rr < .e40 */

rr = MAX(*rr,-);

rr = MIN(*rr,);

rr = exp(*rr);

}

After the UDF that you have defined using DEFINE_HET_RXN_RATE is interpreted or compiled (see

the Fluent Customization Manual for details), the name that you specified in the DEFINE macro argu-

ment (for example, arrh) will become visible and selectable under Reaction Rate Function in the

Reactions tab of the Phase Interaction dialog box. (Note you will first need to specify the Total

Number of Reactions greater than .)

Chapter : Modeling Solidification and Melting

This chapter describes how you can model solidification and melting in ANSYS Fluent. For information

about the theory behind the model, see Solidification and Melting in the Theory Guide. Information

about using the model is organized into the following sections:

.. Setup Procedure

.. Procedures for Modeling Continuous Casting

.. Modeling Thermal and Solutal Buoyancy

.. Solution Procedure

.. Postprocessing

The procedure for setting up a solidification/melting problem is described below. (Note that this pro-

cedure includes only those steps necessary for the solidification/melting model itself; you will need to

set up other models, boundary conditions, and so on, as usual.)

. To use the solidification/melting model, enable the Solidification/Melting option in the Solidification

and Melting dialog box (Figure . :The Solidification and Melting Dialog Box (p. )).

Setup →  Models → Solidification & Melting

Edit...

Figure . : The Solidification and Melting Dialog Box

ANSYS Fluent will automatically enable the energy equation, so you do not have to visit the Energy

dialog box before turning on the solidification/melting model.

. Under Parameters, specify the value of the Mushy Zone Parameter (

in Equation .) as a constant,

or as a user-defined function. Refer to DEFINE_SOLIDIFICATION_PARAMS in the Fluent Customization

Manual for detailed information about the user-defined function.

Values between

and

are recommended for most computations. The higher the value of the

Mushy Zone Parameter, the steeper the damping curve becomes, and the faster the velocity drops

to zero as the material solidifies. Very large values may cause the solution to oscillate as control

volumes alternately solidify and melt with minor perturbations in liquid volume fraction.

. If you want to include the pull velocity in your simulation (as described in Momentum Equations and Pull

Velocity for Continuous Casting in the Theory Guide), enable the Include Pull Velocities option under

. If you are including pull velocities and you want ANSYS Fluent to compute them (using Equation .)

based on the specified velocity boundary conditions, as described in Pull Velocity for Continuous Casting

in the Theory Guide, enable the Compute Pull Velocities option and specify the number of Flow Iterations

Per Pull Velocity Iteration.

Important

It is not necessary to have ANSYS Fluent compute the pull velocities. See Procedures for

Modeling Continuous Casting (p. ) for information about other approaches.

The default value of  for the Flow Iterations Per Pull Velocity Iteration indicates that the pull

velocity equations will be solved after each iteration of the solver. If you increase this value, the pull

velocity equations will be solved less frequently. You may want to increase the number of Flow It-

erations Per Pull Velocity Iteration if the liquid fraction equation is almost converged (that is, the

position of the liquid-solid interface is not changing very much). This will speed up the calculation,

although the residuals may jump when the pull velocities are updated.

. Under Options, select either Lever Rule or Scheil Rule. See Species Equations in the Theory Guide for

details.

Important

The Lever Rule and Scheil Rule options are available only when Species Transport is

enabled in the Species Model dialog box.

. If you select Scheil Rule, then you can enable Back Diffusion. Enter either a constant or a user-defined

function to specify the value of the Back Diffusion Parameter (  in Equation . ). Refer to

DEFINE_SOLIDIFICATION_PARAMS in the Fluent Customization Manual for detailed information about

the user-defined function. Note that the value for the Back Diffusion Parameter must be between  and

.

. In the Create/Edit Materials Dialog Box (p. ) (Figure . :The Create/Edit Materials Dialog Box for Melting

and Solidification (p. )), specify the Pure Solvent Melting Heat (  in Equation . ), Solidus Temperature

(

in Equation . ), and Liquidus Temperature (

in Equation .) for the material being

used in your model.

Setup →

Materials

Modeling Solidification and Melting

Figure . : The Create/Edit Materials Dialog Box for Melting and Solidification

If you are solving for species transport, you need to specify properties for the mixture, including the

method by which the Solidus Temperature and the Liquidus Temperature are calculated. The

default method is the mixing-law (Equation . and Equation . in the Theory Guide), in which

the solidus temperature and the liquidus temperature are calculated from the parameters provided

for each solute (such as the slope of the liquidus line or partition coefficient). However, a user-

defined function of type DEFINE_PROPERTY can be used to specify both of these temperatures.

See the Fluent Customization Manual for examples of DEFINE_PROPERTY.

Important

It is highly recommended that you use the same method for specifying the Solidus

Temperature and the Liquidus Temperature.

When defining the mixture, you will also specify the Mass Diffusivity (

Equation .) and the Eutectic Temperature (

in Equation . ), as well as the Pure Solvent

Melting Heat (  in Equation .) and the Pure Solvent Melting Temperature (

and Equation . ). Note that the solvent is the last species listed under Selected Species in the

Species dialog box.

For each solute, you have to specify the Slope of Liquidus Line (

in the Theory Guide) with respect to the concentration of the solute, the Partition Coefficient (

in Equation . ), the Eutectic Mass Fraction (

in Equation . ), and, if Lever Rule is selected

in the Solidification and Melting dialog box, the coefficient for Diffusion in Solid (

in

Equation . ). It is not necessary to specify

,

,

, and

for the solvent.

Setup Procedure

. Set the boundary conditions.

Setup →

In addition to the usual boundary conditions, consider the following:

If you want to account for the presence of an air gap between a wall and an adjacent solidified region

(as described in Contact Resistance at Walls in the Theory Guide), specify a nonzero value, a profile, or

a user-defined function for Contact Resistance (

in Equation .) under Thermal Conditions in

the Wall Dialog Box (p. ).

If you want to specify the gradient of the surface tension with respect to the temperature at a wall

boundary, you can use the Marangoni Stress option for the wall Shear Condition. See Marangoni

Stress (p. ) for details.

If you want ANSYS Fluent to compute the pull velocities during the calculation, note how your specified

velocity conditions are used in this calculation (see Pull Velocity for Continuous Casting in the Theory

Guide).

Procedures for Modeling Continuous Casting (p. ) contains additional information about modeling

continuous casting. See Solution Procedure (p. ) and Postprocessing (p. ) for information about

solving a solidification/melting model and postprocessing the results.

As described in Momentum Equations and Pull Velocity for Continuous Casting in the Theory Guide,

you can include the pull velocities in your solidification/melting calculation to model continuous casting.

There are three approaches to modeling continuous casting in ANSYS Fluent:

Specify constant or variable pull velocities.

To use this approach (the default), do not enable the Compute Pull Velocities option.

If you use this approach, you will need to patch constant values or custom field functions for the pull

velocities, after you initialize the solution.

Solution →

Solution →

See Patching Values in Selected Cells (p. ) for details about patching values. Note that it is acceptable

to patch values for the pull velocities in the entire domain, because the patched values will be used

only if the liquid fraction,

, is less than .

Have ANSYS Fluent compute the pull velocities (using Equation .) during the calculation, based on the

specified velocity boundary conditions.

To use this approach, enable the Compute Pull Velocities option. This method is computationally

expensive, and is recommended only if the pull velocities are strongly dependent on the location of

the liquid-solid interface.

If you have ANSYS Fluent compute the pull velocities, then there are no additional inputs or setup

procedures beyond those presented in Setup Procedure (p. ).

Have ANSYS Fluent compute the pull velocities just once, and then use those values for the remainder of

To use this approach, perform one iteration with ANSYS Fluent computing the pull velocities, and

then turn off the Compute Pull Velocities option and continue the calculation. For the remainder

of the calculation, ANSYS Fluent will use the values computed for the pull velocities at the first iteration.

When the effects of thermal and solutal buoyancy are present, a flow can be induced inside the domain

due to the effect of gravity on the variable density of the medium. In the case of multi-component so-

lidification problems, the density variation takes place due to temperature changes and also due to

species concentration gradients near the liquid-solid interface. The flow due to buoyancy with solidific-

ation and melting can be modeled in ANSYS Fluent using the thermal and solutal buoyancy options.

For more information on the theory behind buoyancy induced flow in solidification and melting problems,

see Thermal and Solutal Buoyancy in the Theory Guide.

The procedure for setting up a solidification/melting problem is described in Setup Procedure (p. ).

To include thermal and solutal buoyancy effects, perform the following steps:

. Enable the Include Thermal Buoyancy and Include Solutal Buoyancy options in the Solidification

Note

The Include Thermal Buoyancy and Include Solutal Buoyancy options are available

only when solidification is modeled with species transport.

. Define the operating conditions and properties for modeling thermal buoyancy as described in Nat-

ural Convection and Buoyancy-Driven Flows (p. ).

Modeling Thermal and Solutal Buoyancy

. To model solutal buoyancy, specify a value for the Solutal Expansion Coefficient for all the species

except the last one in the mixture in the Create/Edit Materials dialog box.

Note

By default, the eutectic mass fraction of the solute is used as the reference species mass

fraction of the solute for the calculation of the body force due to solutal buoyancy.

Therefore, no additional input is required. However, in certain applications, it is not always

desirable to use the default values of the reference mass fraction. For such cases, the

solute mass fraction values can be entered through text user interface as follows:

define/models/solidification-melting? yes

Include Thermal Buoyancy? yes

Include Solutal Buoyancy? yes

Use reference mass fraction of solutes? yes

Reference mass fraction of the species-i "value"

Before solving the coupled fluid flow and heat transfer problem, you may want to patch an initial

temperature or solve the steady conduction problem as an initial condition. The coupled problem can

then be solved as either steady or transient. Because of the nonlinear nature of these problems, however,

in most cases a transient solution approach is preferred.

You can specify the under-relaxation factor applied to the liquid fraction equation in the Solution

Solution →

Controls

Specify the desired value in the Liquid Fraction Update field under Under-Relaxation Factors. This

sets the value of

in the following equation for updating the liquid fraction from one iteration ( ) to

the next (

):

(.)

where

is the predicted change in liquid fraction.

In many cases, there is no need to change the default value of

. If, however, there are convergence

difficulties, reducing the value may improve the solution convergence. Convergence difficulties can be

expected in steady-state calculations, continuous casting simulations, simulations involving multicom-

ponent solidification, and simulations where a large value of the mushy zone constant is used.

For solidification/melting calculations, you can generate graphical plots or alphanumeric reports of the

following items depending on which other models are enabled in the simulation. These quantities are

available in the Solidification/Melting... category of the variable selection drop-down list that appears

in postprocessing dialog boxes:

Pull Velocity (X, Y, Z, Axial, Radial, and Swirl components)

The Liquid Fraction and Contact Resistivity solution variables are available for all solidification/melting

simulations. The Pull Velocity components are available only if you are including pull velocities (either

computed or specified) in the simulation. Liquidus Temperature and Solidus Temperature are available

only if the Species model is set up to perform a multi-component solidification/melting simulation. See

Field Function Definitions (p. ) for a complete list of field functions and their definitions. Displaying

Figure . : Liquid Fraction Contours for Continuous Crystal Growth (p. ) shows filled contours of liquid

fraction for a continuous crystal growth simulation.

Figure . : Liquid Fraction Contours for Continuous Crystal Growth

Chapter : Modeling Fluid-Structure Interaction (FSI) Within Fluent

This chapter provides details about how to model and simulate one-way and two-way fluid-structure

interaction (FSI) completely within a Fluent session. This is referred to as "intrinsic FSI", as all of the

structural calculations are performed by Fluent; note that you can also use extrinsic solvers for FSI

problems, incorporating the structural data into your Fluent fluid simulation through mapping or system

coupling, as described in Mapping Data for Fluid-Structure Interaction (FSI) Applications (p. ) and

Performing System Coupling Simulations Using Fluent (p. ), respectively. The theoretical aspects of

intrinsic FSI calculations are presented in The Structural Model for Intrinsic Fluid-Structure Interaction

(FSI) in the Theory Guide. The following sections provide details on running intrinsic FSI simulations:

.. Setting Up an Intrinsic Fluid-Structure Interaction (FSI) Simulation

Intrinsic fluid-structure interaction (FSI) capabilities allow you to simulate either one-way or two-way

FSI problems completely within a Fluent session. One-way FSI problems assume that only the fluid side

will have an impact on the solid side through the fluid force that acts on the structure. Since there is

no feedback information from the solid side, for one-way FSI simulations you can either compute the

fluid flow and structural deformation simultaneously, or compute the structural side independently

after the fluid simulation is completed. However, if the solid domain influences the fluid side of the FSI

simulation, then you must model it as a two-way FSI simulation by enabling mesh motion for the fluid

domain through a dynamic mesh.

The solution of an FSI problem requires the solution of both the fluid flow problem as well as the

structural problem. The solution of the structural equations is limited by following:

The structural model only supports quadrilateral and/or triangular cell types in 2D and hexahedral and/or

tetrahedral cell types in 3D.This applies only to the solid zones.

Note

If you use the meshing mode of Fluent to generate a hexcore mesh, the resulting mesh

will not be suitable for the structural model, as such meshes contain small numbers of

polyhedral cells.

The fluid and solid zones must have conformal meshes and be separated by two-sided walls (that is, wall /

wall-shadow pairs).

At least one solid zone must be present in the domain in order to enable the structural model.

The following dynamic mesh options are not supported for intrinsic FSI problems:

– In-Cylinder

– Six DOF

– Contact Detection

The Intrinsic FSI type can only be selected in the Dynamic Mesh Zones dialog box for the side of a two-

sided wall (that is, the wall or wall-shadow) that is immediately adjacent to the fluid cell zone (as indicated

by the Adjacent Cell Zone field in the Wall dialog box).

For a wall that is adjacent to a solid zone or between a solid and fluid zone:

– The only user-defined functions (UDFs) that are supported for displacement and force are

DEFINE_WALL_NODAL_DISP and DEFINE_WALL_NODAL_FORCE, respectively (as described in

DEFINE_WALL_NODAL_DISP and DEFINE_WALL_NODAL_FORCE). All other boundary condition

profiles or UDFs (such as DEFINE_PROFILE) will produce an error message.

– The Shell Conduction option is not supported.

The structural model is not compatible with:

– the 2D Axisymmetric or Axisymmetric Swirl option

– mesh adaption

– overset meshes

– the mesh morpher/optimizer

– British or centimeter-gram-second (CGS) units

– FMG initialization

– adaptive time stepping

The structural model is not available when running Fluent under ANSYS Workbench.

The Linear Elasticity structural model is only appropriate when the stress loading does not exceed the yield

strength of the solid material.

The procedure for setting up an intrinsic FSI simulation is described below. Note that only steps that

are pertinent to the structural model are listed here. You will also need to define the other settings

(such as other material properties, boundary conditions, other models) as usual. For information about

inputs related to other ANSYS Fluent models that you are using in conjunction with the intrinsic FSI

simulation, refer to the appropriate sections for those models.

. (recommended) Launch the double-precision version of ANSYS Fluent.

. Define the settings in the General task page.

Setup →

General

Modeling Fluid-Structure Interaction (FSI) Within Fluent

a.

Define the time dependence of the simulation: one-way FSI problems can be Steady or Transient,

whereas two-way FSI problems must be Transient. Note that modeling two-way FSI is only necessary

when the deformation of the solid zone is significant enough to affect the fluid flow.

b. You can enable the Gravity option and define the coordinates for the acceleration if you would like

the structural model to account for gravitational forces when calculating the deformation of the solid

cell zone.

. Define a solid zone.

Setup →

Note that you can enable the Frame Motion option in the Solid dialog box and define a rotational

velocity for the reference frame if you would like the structural model to account for rotational

forces when calculating the deformation of the solid cell zone. For details, see Defining Zone Mo-

tion (p. ) and Modeling Flows with Moving Reference Frames (p. ).

. For a two-way FSI problem, it is recommended that you run the calculation at this point to obtain a con-

verged solution for the fluid, and then proceed with the following steps to set up and run the structural

model.

. In the Structural Model dialog box, select the Linear Elasticity model.This model enables structural cal-

culations for the solid cell zone such that the internal load is linearly proportional to the nodal displacement,

and the structural stiffness matrix remains constant.

Setup → Models → Structure

Edit...

Figure . : The Structural Model Dialog Box

. Make sure that the material used in the solid cell zone is properly defined, by setting the Youngs Modulus

and Poisson Ratio fields in the Properties group box of the Create/Edit Materials dialog box.

Setup →

Materials

. If you plan to define the displacement or force applied to the nodes of a wall adjacent to the solid zone

using a user-defined function (UDF), interpret or compile a suitable UDF. For details, see

DEFINE_WALL_NODAL_DISP or DEFINE_WALL_NODAL_FORCE, respectively.

. For every wall that is immediately adjacent to the solid zone, define the displacement boundary condition

settings in the Structure tab of the Wall dialog box.

Setting Up an Intrinsic Fluid-Structure Interaction (FSI) Simulation

Setup →

Figure . : The Structure Tab of the Wall Dialog Box

The walls will be one-sided when they are only adjacent to a solid cell zone, and will be two-sided

(that is, a wall / wall-shadow pair) when they are adjacent to both a solid and a fluid cell zone. Note

that for two-sided walls, the Structure tab is only available for one side of the wall / wall-shadow

pair; which one will depend on how the mesh was set up.

You must select one of the following from the X-, Y-, and (for 3D cases) Z-Displacement Boundary

Condition drop-down lists, in order to define how the displacement is calculated for the nodes in

that particular direction:

Stress Free specifies that the displacement is not affected by stress loads from the fluid flow.

Node X-, Node Y-, and (for 3D cases) Node Z-Force specifies that the displacement results from a specified

force applied on the nodes, which is defined using the Node X-, Node Y-, and (for 3D cases) Node Z-

Force field.

Node X-, Node Y-, and (for 3D cases) Node Z-Displacement applies a specified displacement on the

nodes, which is defined using the X-, Y-, and (for 3D cases) Z-Displacement field.

Face Pressure specifies that the displacement results from a specified pressure load applied on the

faces, which is defined using the Face Pressure field.

Intrinsic FSI specifies that the displacement results from pressure loads exerted by the fluid flow on the

faces. Note that this selection is only available for a zone that is part of a wall / wall-shadow pair.

Figure . : The Wall Dialog Box for a Two-Sided Wall

. For two-way FSI simulations, define dynamic mesh properties to allow the mesh to handle the deformation

of the solid zone.This includes the following:

Enable dynamic mesh Smoothing, and select either the Diffusion or Linearly Elastic Solid method in

the Mesh Method Settings Dialog Box (p. ).

For cases with strong FSI coupling (such as when the fluid and solid densities are comparable), enable

the Implicit Update option in the Dynamic Mesh task page and define appropriate settings in the Im-

plicit Update tab of the Options dialog box. For details, see Setting Dynamic Mesh Modeling Paramet-

ers (p. ) and Implicit Update Settings (p. ).

Define an Intrinsic FSI dynamic mesh zone for the side of a two-sided wall (that is, the wall or wall-

shadow) that is immediately adjacent to the fluid cell zone (as indicated by the Adjacent Cell Zone field

in the Wall dialog box). For further details, see Intrinsic FSI Motion (p. ).

Setup →

. For transient simulations, you can make a selection from the Structure Transient Formulation

drop-down list in the Solution Methods Task Page (p. ) to specify the direct time integration

method used to solve the finite element semi-discrete equation of motion. You can select from the

Newmark method (default) or the Backward Euler method. For further details about these methods,

see Dynamic Structural Systems in the Theory Guide.

Solution →

Methods

. You can revise the following settings if you find that the defaults do not produce satisfactory results:

You can specify the solution method used by the linear solver for the structural model calculations. By

default, the bi-conjugate gradient stabilized (BCGSTAB) method is used.This method offers a good balance

of speed and robustness. If divergence is detected with BCGSTAB, then the generalized minimal residual

(GMRES) method will be used for an iteration as a fallback, and you will be informed in the console that

a "fe-structure" equation is being stabilized to enhance linear solver robustness. If you find that your

residual level / drop is not satisfactory, you can try increasing the maximum number of inner iterations

from the default of  by using the following text command:

define → models → structure → controls → max-iter

If the BCGSTAB method continues to produce unsatisfactory residuals with a higher number of

inner iterations or if you repeatedly see console messages that say the GMRES fallback is being

used, you can change the solution to the GMRES method. Note that GMRES is the most robust

method, but it is also more demanding in terms of memory usage and solver time. With GMRES,

it is recommended that you start with the maximum iterations set to . Also available is the

conjugate gradient (CG) method: while in some cases it is the least robust method, it can result

in faster calculations, as it takes advantage of the symmetry of the matrix used in the linear systems

of equations. To change the solution method, use the following text command:

define → models → structure → controls → amg-stabilization

For transient simulations, you can revise the numerical damping factor for the structural model calculations

(that is, the amplitude decay factor  in Equation . in the Theory Guide) by using the following text

command:

define → models → structure → controls → numerical-damping-factor?

You can enable an explicit fluid-structure interaction force by using the following text command:

define → models → structure → expert → explicit-fsi-force?

You can enable the inclusion of operating pressure into the fluid-structure interaction force by using

define → models → structure → expert → include-pop-in-fsi-force?

You can enable the inclusion of a viscous fluid-structure interaction force by using the following text

command:

define → models → structure → expert → include-viscous-fsi-force?

. If necessary, revise the default convergence criteria for the x- y-, and (for 3D cases) z-displacement residual

equations in the Residual Monitors Dialog Box (p. ).

Solution → Monitors → Residual

Edit...

. (Optional) Create structural point surfaces at points of interest within the solid zone, which you can

use for monitoring and reporting data. Note that for two-way FSI simulations, a structural point

surface does not necessarily remain fixed in space, but will continue to represent its original cell as

the solid zone moves / deforms.

Results → Surfaces

New → Structural Point...

For further details, see Structural Point Surfaces (p. ).

To monitor a field variable at such a structural point surface, create a report definition. For example,

you could monitor and plot the vertex average of the displacement of the nodes that surround a

structural point surface:

Solution → Report Definitions

New → Surface Report → Vertex Average...

For further details, see Creating Report Definitions (p. ).

. Initialize the solution. Note that for standard initialization, you can specify the initial X, Y, and (for 3D cases)

Z Displacement in the Solution Initialization Task Page (p. ).

Solution →

. Run the calculation.

Solution →

Tip

For one-way FSI simulations, the calculation time will be faster if you first run the calcu-

lation with only the fluid equations enabled in the Equations dialog box, and then run

it with only the structure equation enabled.

. View the results by displaying contours of the following field variables (in the Structure... category):

X, Y, and Z Displacement for the displacement values

Sigma XX, YY, XY, ZZ, YZ, and XZ for the stress tensor values

New...

Note

You should confirm that the stress loading does not exceed the yield strength of the

solid material, as this is an assumption of the Linear Elasticity structural model.

New...

Note

Chapter : Modeling Eulerian Wall Films

The Eulerian Wall Film (EWF) model can be used to predict the creation and flow of thin liquid films on

the surface of walls. This chapter presents information about the basic functionality of the Eulerian Wall

Film (EWF) model. Additional information about the model is provided in the following sections:

.. Setting Eulerian Wall Film Model Options

.. Setting Eulerian Wall Film Solution Controls

.. Setting Eulerian Wall Film Boundary, Initial, and Source Term Conditions

.. Postprocessing the Eulerian Wall Film

For more information about Eulerian Wall Film model theory, see Eulerian Wall Films in the Theory

Guide (p. ). For more information about setting boundary conditions for liquid films at wall boundaries,

see Wall Film Conditions for Walls (p. ).

The following limitations exist for the Eulerian Wall Film model:

The Eulerian Wall Film model is available for 3D geometries only.

Many models (for example,VOF multiphase flow or radiation) will not interact correctly with the film model

without first modifying the boundary conditions using UDFs.

Wallfilm behavior at junctions with baffles (zero-thickness walls) may lead to unphysical results due to the

local mesh topology (wall, wall-shadow) and should be used with care, that is, isolated film walls must not

share a common edge.

The wall film can only be single-component, but not multi-component.

The Eulerian Wall Film model is not compatible with non-conformal interfaces.

The Eulerian Wall Film model is not compatible with mesh operations in Fluent (such as mesh adaption, cell

separation, face zone extrusion, and cell zone type change).

You can enable the Eulerian Wall Film model by selecting Eulerian Wall Film from the Models task

page.

Setup → Models → Eulerian Wall Film

Edit...

This opens the Eulerian Wall Film dialog box.

Once you open the Eulerian Wall Film Dialog Box (p. ), you can select the Eulerian Wall Film check

box to enable the model so that you can use it in your simulation. Enabling the model expands the

dialog box to reveal additional model options and solution controls.

Important

If you want to modify your mesh in Fluent, you must first disable the Eulerian Wall Film

model. Once you save the modified mesh, you must re-enable the Eulerian Wall Film model

and re-initialize your case.

You can set general Eulerian Wall Film model options in the Model Options and Setup tab of the Eu-

lerian Wall Film dialog box. This tab contains controls for specific solution, discrete phase model (DPM),

and material options for the Eulerian Wall Film model.

Modeling Eulerian Wall Films

In the Model Options and Setup tab, the following options and controls are available:

Solve Momentum

specifies whether the momentum equation (see Equation . in the Fluent Theory Guide) is solved for the

wall film or not. In the Momentum Options group box, you can individually select each term of the

equation for inclusion in the calculations.

Note that Spreading Term and Surface Tension under Momentum Options are available only

when Pressure Gradient is selected.

Solve Energy

specifies whether the energy equation (see Equation . in the Fluent Theory Guide) is solved for the wall

film or not.

Setting Eulerian Wall Film Model Options

Solve Scalar

specifies whether the passive scalar transport equation Equation . is solved for the wall film or not.

When the Solve Scalar option is enabled, you can specify Scalar Diffusivity.

DPM Collection

includes discrete phase particles and their interaction with the film model (see DPM Collection in the Fluent

Theory Guide).You can select:

Particle Splashing

You can specify splashing options in the Wall Film tab of the Wall dialog box. For details, see

Setting Eulerian Wall Film Boundary, Initial, and Source Term Conditions (p. ).

Particle Stripping and specify the settings under the Stripping Options group box (for details, see

Film Separation in the Fluent Theory Guide)

Edge Separation and specify the settings under the Separation Options group box (for details, see

Note that Random Separation means that the locations at which the newly spawned particles

are injected (due to film separation) are randomly selected along the edge at which the separation

takes place.

Treat Sharp Edge

accounts for the effects of sharp edges and specify Sharp Edge Angle.When the Treat Sharp Edge option

is enabled and where the edge angle is smaller than the Sharp Edge Angle, the film wall edge is treated

as a boundary edge (namely, the film becomes detached from the wall, rather than bending around the

edge and attaching to the wall). If the Discrete Phase Model has been enabled along with the Eulerian

Wall Film model, then the film wall edge is treated as a separation edge.

Phase Accretion

accounts for the effect of the interaction of the wall film with Eulerian and Mixture multiphase flow (see

Secondary Phase Accretion in the Fluent Theory Guide).This option enables you to compute the secondary

phase collection efficiency on a wall surface.This option is only available when the Eulerian or Mixture

(with Slip Velocity) Multiphase model is enabled.

Note

The following considerations should be taken into account when the Eulerian Wall Film

model is used with the Eulerian or Mixture multiphase models:

You must create temporary placeholder injections in order to model edge separation

and edge stripping.

The material properties for the secondary phase should be the same as the DPM

The name of the secondary phase material should be included in the name of the DPM

particle’s material and should be appended with the string ‘-particle’ (for example, if

the secondary phase material name is waterliquid- eulerian, then the DPM particle’s

material name should be waterliquid-eulerian-particle).

Phase Change

accounts for phase changes between the film material (liquid) and the gas species (vapor) (see Coupling

of Wall Film with Mixture Species Transport in the Fluent Theory Guide).This option enables you to set the

Film Vapor Material—in the Material Options group box.

Phase change parameters—in the Wall Film tab of the Wall dialog box. For details, see Setting Eulerian

Wall Film Boundary, Initial, and Source Term Conditions (p. ).

Note

The liquid film can only be a single-component fluid. The secondary phase that is intended

for the film material cannot be a mixture of species.

Material Options

allow to select film material and film vapour material (available only for Phase Change calculations) and

specify wall film surface tension.

Note

The type of material for a wall film must be Fluid, Droplet Particle, or Inert Particle

(fluid).

You can define density, viscosity, specific heat, thermal conductivity, vaporization tem-

perature, and vapor saturation pressure of a wall film material or film vapor using one

of the following methods:

constant

polynomial (including piecewise linear and piecewise polynomial)

compressible liquid (for fluid density)

user-defined (not available for fluid specific heat)

default-method (for film vapor saturation pressure)

Solve Wall Film

enables you to skip the wall film solution during the gas phase solution, but keep the variables and setup

active.

Note

The wall film cannot be solved without first initializing the wall film model (using

the Initialize button) to initialize the wall film variables and prepare the solver for

the solution procedure.

You can also use the define/models/eulerian-wallfilm/model-options text command to

define the settings and the discretization methods for the Eulerian Wall Film model.

You can set solution controls for the Eulerian Wall Film model in the Solution Method and Control

tab of the Eulerian Wall Film dialog box. This tab contains controls for specific temporal and spatial

discretization options for the Eulerian Wall Film model.

Figure . : Eulerian Wall Film Solution Controls (Steady Flow)

Figure . : Eulerian Wall Film Solution Controls (Unsteady Flow)

In the Solution Method and Control tab, you can set the following:

Temporal and spatial (continuity, momentum, energy, and passive scalar) discretization methods under

Discretization.

Maximum Thickness for the film.

The Maximum Thickness setting will limit the film thickness by removing material from the film

where this value is exceeded.

Setting Eulerian Wall Film Solution Controls

For steady state calculations (Figure . : Eulerian Wall Film Solution Controls (Steady Flow) (p. )):

You can specify the film model specific Time Step (the Eulerian Wall Film model is always tran-

sient), or you can select the Adaptive Time Stepping option to set the Max. Courant Number

and the Initial Time Step (see Steady Flow).

For transient cases (Figure . : Eulerian Wall Film Solution Controls (Unsteady Flow) (p. ):

You can define the Number of Time Steps per main flow time step and the Sub-Time Report

Interval for film calculation reporting. Note that the first and the last sub-time steps are always

reported.

For either first or second order implicit time discretization calculations:

You can control the number of film Sub-Iterations, the value of Sub-Iteration Stop below which

reported.

the film sub-iteration stops, and the Sub-Iter Report Interval for film sub-iteration reporting.

Note that the first and the last sub-iterations are always reported.

If DPM Collections is selected in the Model Options and Setup tab:

You can set how often the DPM phase is calculated for the film by specifying a value for the

Film Steps per DPM Step These controls are only available if Interaction with Continuous

Phase is disabled in the Discrete Phase Model dialog box.

.. Setting Eulerian Wall Film Boundary, Initial, and Source Term Con-

ditions

In the Wall dialog box, under the Wall Film tab, you can set boundary, initial, and source term conditions

for liquid films on specified wall boundaries. When you select the Eulerian Film Wall option, Fluent

solver designates the wall as a film wall. Wall film equations are only solved on designated film walls.

Figure . : Wall Dialog Box (Initial Conditions)

The following types of film conditions exist in ANSYS Fluent:

Boundary Condition: Is where film mass, momentum, energy and scalar quantities are introduced to the

wall film solution domain.

You can enter values for the following quantities:

Setting Eulerian Wall Film Boundary, Initial, and Source Term Conditions

– Film Mass Flux

– X-Momentum Flux, Y-Momentum Flux, and Z-Momentum Flux

– Incoming Film Temperature

– Film Passive Scalar Flux

For moving wall simulations, you can specify the film momentum flux relative to the wall on which

liquid film is defined by selecting Relative Film Momentum Flux. Note that this option is only

available when Moving Wall is selected in the Wall dialog box and/or Frame Motion is selected in

the Fluid dialog box.

the film momentum flux or initial velocity inputs will be relative to the wall on which liquid film is

defined.

Initial Condition: Is the initial state of wall film.

You can set values for the following quantities:

– Film Height

– X-Velocity, Y-Velocity, and Z-Velocity components

– Film Temperature

– Film Passive Scalar

For moving wall simulations, you can specify the initial velocity relative to the wall on which liquid

film is defined by selecting Relative Initial Film Velocity. Note that this option is only available when

Moving Wall is selected in the Wall dialog box and/or Frame Motion is selected in the Fluid dialog

box.

If you select the User Source Terms option (available only with initial condition), you can also specify

additional source terms to the film continuity, momentum, energy, and passive scalar equations by

setting values for the following quantities:

– Mass Flux

– Heat Flux

– Scalar Flux

For both boundary and initial conditions, if you select the Flow Momentum Coupling option, the liquid

film and the gas flow shares the same velocity at the interface of the liquid-gas interface using a two-

way coupling. If you clear this option, the coupling between the liquid film and the gas flow occurs

only one-way, namely, while the gas flow impacts the film flow, the film flow does not impact the bulk

of the gas flow.

When the Phase Change option is selected in the Eulerian Wall Film dialog box, you can enable the

Film Phase Change for the selected film wall, and then select the Phase Change Model and specify

the model parameters. The following phase change models are available:

diffusion-balance

For the diffusion-balance model, you can specify Condensation Constant and Vaporization Con-

stant.

wall-boundary-layer

No user input is required for this model.

For the user-defined model, you can specify Condensation Rate and Vaporization Rate as constants,

parameters, or profile user-defined functions (UDFs). Note that condensation and vaporization rates

must be specified as positive values in kg/s. For more information on profile UDFs, the separate Fluent

For more information on the phase change models see Coupling of Wall Film with Mixture Species

Transport in the Fluent Theory Guide.

For cases with initial condition, if you select the Surface Tension option in the Eulerian Wall Film

dialog box, then you can enable the Partial Wetting model for the selected film wall by selecting the

Film Contact Angle option. You can then specify the following parameters in the Contact Angle

Parameters group box:

Mean Contact Angle (

in Partial Wetting Effect in the Fluent Theory Guide)

The input range for the mean Contact Angle is  to  degrees. You can also use a user-defined

profile UDF. The UDF must return a contact angle value within the above range in radian. For more

information on profile UDFs, the separate Fluent Customization Manual.

Relative Standard Deviation (  in Partial Wetting Effect in the Fluent Theory Guide)

The input for the Relative Standard Deviation should be in the range of  to %.

Contact Angle Force Beta (  in Equation . in the Fluent Theory Guide)

The input range for Contact Angle Force Beta is  to .

For more information on modelling film partial wetting effect see Partial Wetting Effect in the Fluent

When the DPM Collection option is selected in the Eulerian Wall Film dialog box, you can select a

particle-wall impingement model and specify relevant model parameters in the Wall dialog box. The

following impingement models are available in ANSYS Fluent:

stanton-rutland (see The Stanton-Rutland Model in the Fluent Theory Guide for details)

kuhnke (see The Kuhnke Model in the Fluent Theory Guide for details)

For the Kuhnke model, you must specify the following model parameters:

– Ra:The wall mean roughness that is used to compute

– Rz:The average surface roughness that is used to compute splashed particle reflection angle distribution

Equation . in the Fluent Theory Guide.

– Critical Temperature Factor:The dimensionless variable that is used to determine the impingement

regime transition temperature in Equation . in the Fluent Theory Guide.

Note

You can also add an impingement effect via UDFs as described in Hooking DEFINE_IM-

PINGEMENT UDFs, Hooking DEFINE_FILM_REGIME UDFs, and Hooking

DEFINE_SPLASHING_DISTRIBUTION UDFs in the Fluent Customization Manual. Note that

UDFs settings will override those for the impingement/splashing model selected for the Eu-

lerian wall film boundary condition.

In addition, when Particle Splashing is selected in the Eulerian Wall Film dialog box, you can select

DPM Wall Splash and specify Number of Splashed Particles.

When using the Eulerian Wall Film model, the following additional variables will be available for post-

processing (see Field Function Definitions (p. ) for their definitions):

Film Mass

Film Temperature (when Solve Energy is enabled)

Film X-Velocity

Film Y-Velocity

Film Z-Velocity

Film Surface X-Velocity

Film Surface Y-Velocity

Film Surface Z-Velocity

Film Surface Temperature (when Solve Energy is enabled)

Film Passive Scalar (when Solve Scalar is enabled)

Film Density (when film material density is non-constant)

Film Coverage (when Solve Momentum is enabled)

Film Stripped Mass (when Particle Stripping is enabled)

Film Stripped Diam (when Particle Stripping is enabled)

Film DPM Mass Source (when DPM Collection is enabled)

Film DPM Energy Source (when DPM Collection and Solve Energy are enabled)

Film DPM X-Momentum Source (when DPM Collection is enabled)

Film DPM Y-Momentum Source (when DPM Collection is enabled)

Film DPM Z-Momentum Source (when DPM Collection is enabled)

Film Separated Mass (when Edge Separation is enabled)

Film Separated Diam (when Edge Separation is enabled)

Film Separation Rate (when Edge Separation is enabled)

Film Phase Change Rate (when Phase Change is enabled)

Film Secondary Phase Mass (when Phase Accretion is enabled)

Film Secondary Phase Collection Coef (when Phase Accretion is enabled)

You can report on the mass and energy fluxes for the Eulerian Wall Film model using the Flux Reports

dialog box (see Generating a Flux Report (p. )), for domain boundaries such as inlets, outlets, and so

on, as well as wall boundaries.

Edit...

The Film Mass Flow Rate and Film Heat Transfer Rate are available as options in the Flux Reports

dialog box when the Eulerian Wall Film model is enabled.

Note

The energy flux report only accounts for the heat transfer rate through the external boundary.

It does not consider heat transfer at gas-liquid interfaces or heat transfer due to phase change

or film-DPM interaction.

You can also report on the mass flow rate and heat transfer rate using the User Interface (TUI) as follows:

For mass flow rate, enter the text command report/fluxes/film-mass-flow.

For heat transfer  rate, enter the text command report/fluxes/film-heat-transfer.

You will be prompted for the boundary face zone IDs for which the report will be generated, and

whether or not you want to save the reported values to a file. ANSYS Fluent will either print the report

in the console or write it to the file you have specified.

Postprocessing the Eulerian Wall Film

Chapter : Modeling Electric Potential Field

This chapter provides details about how to model and simulate the electric potential field in ANSYS

Fluent. The theoretical aspects of the electric potential model are presented in Electric Potential in the

Fluent Theory Guide. Additional information about the model is provided in the following sections:

.. Using the Electric Potential Model

.. Postprocessing the Electric Potential Field

The ANSYS Fluent electric potential model allows for predicting the electric potential field and its effects.

The electric potential model can be used separately (for example, to compute electric static force for

charged particles in a DPM calculation) or in combination with other ANSYS Fluent models.

The electric potential solver has been integrated with the electrochemical reaction model (Electrochem-

ical Reactions in the Fluent Theory Guide). When you enable the electrochemistry in your case, ANSYS

Fluent automatically enables the electric potential solver. However, if you want to use the electric po-

tential model along with other ANSYS Fluent models, you need to manually enable it as described in

Using the Electric Potential Model (p. ).

Using the electric potential solver, you can simulate the electric potential field in both fluid and solid

zones.

When defining the boundary conditions for the electric potential field, you can specify either potential

or current density at the external walls.

The following limitation exist for the electric potential model:

The electric potential model cannot be used in simulations with walls that have a shell conduction boundary

The procedure for setting up the electric potential model is described below. Note that only steps that

are pertinent to electric potential field modeling are listed here. You will also need to define the other

settings (such as other material properties, boundary conditions, other models) as usual. For information

about inputs related to other ANSYS Fluent models that you are using in conjunction with the electric

potential model, refer to the appropriate sections for those models.

. In the Potential dialog box, which is opened from the Model/Electric Potential tree item, enable the

Potential Equation option.

Once the Potential Equation is enabled, the electric conductivity material property for fluid, solid,

and mixture materials defined in your case will appear in the Create/Edit Materials dialog box.

. If you want to include Joule heating in the energy equation (Equation . in the Fluent Theory Guide), under

the Model Option group box, enable Include Joule Heating in Energy Equation.

Note

The Include Joule Heating in Energy Equation option appears in the Potential dialog

box only when Energy Equation is enabled in the Energy dialog box.

. In the Create/Edit Materials dialog box, under Properties, specify Electric Conductivity for the conductive

materials defined in your simulation.

Setup →

Materials

. Define boundary conditions on conductive external walls.

Setup →

Modeling Electric Potential Field

For one-sided walls, you can specify the following conditions at the boundary wall:

Setup →

Contact Resistance: is  in Equation . in the Fluent Theory Guide

One of the following potential boundary conditions:

– Current Density (if Specified Flux is selected from the Potential Boundary Condition drop-down

list)

– Potential (if Specified Value is selected from the Potential Boundary Condition drop-down list)

For two-sided internal walls, the coupled boundary treatment is always applied to wall and wall-

shadow pairs. In addition, you can apply contact resistance to internal walls. Note that you only

need to define Contact Resistance on one of the walls. The value you specify on one wall will be

automatically copied to another wall.

. If required, specify electric potential conditions on other boundaries in the Potential tab of the boundary

conditions dialog boxes. Note that the default setting, zero current flux, is suitable for most problems and

needs not be changed.

. If you want to fix a value of potential or specify a potential source in a cell zone, you can do it by setting

the Fixed Values or Source Terms in the appropriate cell zone condition dialog box.

For potential field calculations, you can generate graphical plots or alphanumeric reports of the following

items (see Field Function Definitions (p. ) for their definitions). These quantities are available in the

variable selection drop-down lists that appear in postprocessing dialog boxes:

Electric Potential (in the Potential... category)

Electric Conductivity (in the Properties... category)

Current Magnitude (in the Potential... category)

Joule Heat Source (in the Potential... category)

You can also generate vector plots of the electric current fields by selecting Electric Current in the

Vectors of drop-down list inVectors Dialog Box (p. ).

Postprocessing the Electric Potential Field

Chapter : Modeling Batteries

This chapter provides information about using the battery models available in ANSYS Fluent. Additional

information about the model is provided in the following sections:

.. Using the Single-Potential Empirical Battery Model

.. Using the Dual-Potential MSMD and Cell Network Battery Models

The application of lithium ion batteries has been rapidly expanding from electric appliances and elec-

tronic devices to hybrid electric vehicles (HEVs) and electric vehicles (EVs), due to their high energy

density. The main concerns when designing a Li-ion battery are its performance, life, and safety. The

ANSYS Fluent battery models allow simulating a single battery cell or a battery pack using CFD technology

to study their thermal and electrochemical behavior. The ANSYS Fluent battery models are provided as

add-on modules with the standard ANSYS Fluent licensed software.

Note that the Fluent Tutorials provides tutorials that illustrate how to use the ANSYS Fluent battery

models.

This chapter contains the following information:

... Overview

... General Procedure

... Installing the Battery Module

In a lithium-ion battery, the anode and cathode are made of active materials coated on the surface of

metal foils. A polymer separator is placed between the foils of opposite polarity to prevent electrons

from passing between them. To predict the evolution of the chemical, thermal, and electrical processes

in a battery, ANSYS Fluent offers the following models:

Using the Single-Potential Empirical Battery Model (p. )

Using the Dual-Potential MSMD and Cell Network Battery Models (p. )

The Single-Potential Empirical Battery Model is useful if the geometries of the current collector, elec-

trodes, and separator can be fully resolved. One potential equation is solved in the computational

domain. This model is best suited for electrode-scale predictions in a single battery cell.

The model, however, has a limited ability to study the full range of electrochemical phenomena in

battery systems, especially systems having complex geometry. When constructing a battery cell, the

anode-separator-cathode sandwich layer is usually wound or stacked up into a 'jelly roll' or a prismatic

shape. It would be very expensive to resolve all the layers explicitly, even for a single battery cell.

Furthermore, many industrial applications use a battery pack consisting of a large number of cells

connected in series or in parallel.

The ANSYS Fluent Dual Potential Multi-Scale Multi-Dimensional (MSMD) Battery model overcomes

these limitations by using a homogeneous model based on a multi-scale multi-dimensional approach.

In this approach, the whole battery is treated as an orthotropic continuum; thus, the mesh is no longer

constrained by the micro-structure of the battery. Two potential equations are solved in the battery

domain. To fit various analysis needs, the model includes three electrochemical submodels, namely,

the Newman, Tiedemann, Gu, and Kim (NTGK) empirical model, the Equivalent Circuit model (ECM),

and the Newman’s Pseudo-2D (P2D) model having different level of complexity. The model offers you

the flexibility to study the physical and electrochemical phenomena that extend over many length

scales in battery systems of various arrangements.

The following describes an overview of the procedure required in order to use the Battery Model in

. Start ANSYS Fluent.

. Scale the grid, if necessary.

. Load the module and use the Battery Model dialog box to define the battery model parameters.

. Define material properties.

. Set the operating conditions.

. Start the calculations.

. Save the case and data files.

. Process your results.

Important

Note that the majority of this manual describes how to set up the ANSYS Fluent Battery

Model using the graphical user interface. You can also perform various tasks using the text

The battery add-on modules are installed with the standard installation of ANSYS Fluent in a directories

called addons/battery (for the single-potential empirical battery module) and addons/msmdbatt

(for the dual-potential MSMD battery model) in your installation area. The battery modules consist of

UDF libraries and pre-compiled scheme libraries that need to be loaded and activated before calculations

can be performed. A number of UDFs are used to solve the battery equations. Once you loaded the

battery add-on module, UDF and scheme libraries that are required by the battery model are automat-

ically loaded. Further details are provided in chapters that describes the models.

Modeling Batteries

The procedure for setting up and solving the Single-Potential Empirical battery model is described in

detail in this section. Refer to Single-Potential Empirical Battery Model Theoryfor information about the

theory.

... Geometry Definition for the Single-Potential Empirical Battery Model

... Loading the Single-Potential Empirical Battery Module

... Getting Started With the Single-Potential Empirical Battery Model

... Solution Controls for the Single-Potential Empirical Battery Model

... Postprocessing the Single-Potential Empirical Battery Model

... User-Accessible Functions

For information about inputs related to other models used in conjunction with the battery model, see

the appropriate sections for those models in the ANSYS Fluent Fluent User's Guide (p. ).

Due to the fact that there are a number of different physical zones associated with the battery cell,

the following regions must be present in the battery mesh:

Anode

Cathode

Separator (‘zero’ thickness wall/wall-shadow interface)

Note

For electro-chemical types of simulation, 3D double-precision is recommended.

The single-potential empirical battery add-on module is installed with the standard installation of

ANSYS Fluent in a directory called addons/battery in your installation area. The battery module

consists of a UDF library and a pre-compiled Scheme library, which need to be loaded and activated

before calculations can be performed.

The battery module is loaded into ANSYS Fluent through the text user interface (TUI). The module can

be loaded only when a valid ANSYS Fluent case file has been set or read. The text command to load

the module is

. none

. MHD Model

Using the Single-Potential Empirical Battery Model

Select the single-potential battery model by entering the module number . During the loading process,

a Scheme library containing the graphical and text user interface, and a UDF library containing a set

of user-defined functions (UDFs) for the battery module are loaded into ANSYS Fluent. This is reported

to the console. The UDF library also becomes visible as a new entry in the UDF Library Manager

dialog box. The basic setup of the battery model is performed automatically when the battery module

is successfully loaded.

The battery model is implemented by user-defined functions (UDFs) and scheme routines in ANSYS

Fluent. A number of UDFs are used to solve the battery equations. When you loaded the battery add-

on module in the previous step (Loading the Single-Potential Empirical Battery Module (p. )), UDF

and scheme libraries that are required by the battery model were automatically loaded. Before you

can begin the process of defining your battery model, however, you will need to perform some addi-

tional setup tasks that involve allocating user-defined memory for the UDFs and hooking an adjust

UDF to ANSYS Fluent. Follow the procedure below.

Once the module has been loaded, in order to set battery model parameters and assign properties to

the relevant regions in your battery, you need to access the battery graphical user interface (the Battery

Model dialog box).

To enable the battery model: In the Outline View under the Models branch, right-click Battery

Model and click Edit... in the menu that opens.

Setup → Models → Battery Model

Edit...

Figure . : The Battery Model Option in the Outline View

This opens the Battery Model dialog box.

Once you open the Battery Model dialog box, you can select the Enable Battery Model check box

to enable the model so that you can use it in your simulation. Enabling the model expands the dialog

box to reveal additional model options and solution controls.

The Model Parameters tab of the Battery Model dialog box allows you to access general model settings

when solving a battery problem. Likewise, the Separator tab allows you to set options for the battery

separator. Finally, the Electric Field tab allows you to set parameters for the electric field. For additional

information, see the following sections:

.... Specifying Single-Potential Empirical Battery Model Parameters

.... Specifying Separator Parameters

.... Specifying Electric Field Parameters

The Model Parameters tab of the Battery Model dialog box allows you to turn on or off various

options when solving a battery problem.

Figure . : The Battery Model Dialog Box (Model Parameters Tab)

In the Model Parameters tab, you can set various model options, solution controls, electrical para-

meters, as well as activation parameters.

For Model Options, you can:

Enable Joule Heat Source in order to include the Joule Heating source in the thermal energy equation

(Equation . ). (enabled by default)

Enable E-Chem Heat Source in order to include the heat source due to electrochemistry in the thermal

energy equation (Equation . ). (enabled by default)

Enable Separator Submodel in order to specify your own values for the Separator Thickness and Res-

istivity, instead of the Y Coefficients, for modeling the separator. Note that when this option is selected,

the inputs for the Y Coefficients are grayed out, and the Separator Property fields are active in the

Separator tab.

Note

The separator submodel is provided as an alternative method to calculate the separator

resistance. When the option is enabled, the separator resistance is computed as R =

(separator resistivity)*(separator thickness), where separator resistivity and separator thickness

are supplied by you. When the option is disabled (the default), the separator resistance

is computed by

For Solution Controls, you can set the Current Under-Relaxation Factor.

For Electrical Parameters, you can set the Nominal Capacity (the capacity of the battery cell). If you

select Fixed DoD (for steady state simulation only), then you can specify a Nominal DoD value (depth

of discharge). For the Solution Options, if you select:

Specified C-Rate, you can set a value for the Discharge C-Rate (the hourly rate at which a battery

is discharged). In this case, the total current at the cathode tabs are fixed as the product of C-Rate

and Nominal Capacity, while the electrical potential is anchored at zero on the anode tabs.

Specified System Current, you can set a value for the total current (applied to the anode tabs). In

this case, the electrical potential is set to zero at the anode tabs.

Specified System Voltage, you can set a value for the System Voltage (applied to the cathode tab;

the anode tab has a voltage of  V).

Set in Boundary Conditions, you can set the UDS boundary conditions directly, for example, the

voltage value or the current value (specified flux), using the Boundary Conditions task page in ANSYS

Fluent for the specific face zone.

Note

When the steady state solver is used, the Fixed DoD option has to be selected. Al-

ternatively, the transient solver can be used to analyze variable DoD problems.

For Activation Parameters, you can specify the U Coefficients for Equation . and the Y Coefficients

for Equation . (if the Enable Separator Submodel option is disabled).

Note

The coefficient values for the Activation Parameters are based on battery cell polarization

test curves. Obtaining coefficient values (other than the default values) can be dependant

on your battery configuration and material properties. For more information about coeffi-

cient values, refer to the work performed by Gu . You will likely need to make adjust-

ments (for example, if you are modeling lithium ion batteries) when using your own exper-

imental data.

You can also specify the Temperature Corrections, if needed, though the default values are suitable

in most cases. The temperature corrections provide additional accuracy to account for local temper-

ature effects, and correspond to the temperature terms in Equation . and Equation ..

The Separator tab of the Battery Model dialog box allows you to select interfaces as the Anode

Separator, the Cathode Separator, as well as the Separator Properties, if appropriate.

Figure . : The Battery Model Dialog Box (Separator Tab)

In the Separator tab, specify the zones for the Anode Separator and the Cathode Separator. If the

Enable Separator Submodel option is selected in the Model Parameters tab, you can specify the

Separator Properties such as the Separator Thickness and the Separator Resistivity.

The Electric Field tab of the Battery Model dialog box allows you to set the properties of the Con-

ductive Regions, Contact Surfaces, and the External Connectors.

Figure . : The Battery Model Dialog Box (Electric Field Tab)

In the Electric Field tab, specify the zones for the Conductive Regions and the Contact Surfaces

(as well as the Contact Resistance) for any selected contact surface. In addition, you can specify the

anode and cathode tap surfaces for the External Connectors of the battery.

When you use the Battery model, the electric potential equation is solved in addition to other fluid

dynamic equations, depending on the type of simulation. The electric potential equation is listed as

one of the solved equations by ANSYS Fluent in the Equation dialog box, where it can be enabled/dis-

abled in the solution process.

Solution →

Also, keep in mind the Advanced Solution Controls dialog box, where you can set the multigrid cycle

type for the electric potential equation, if required.

Setup →

Controls → Advanced...

Note

When choosing a solution method for your simulation, the Least Squares Cell Based gradient

spatial discretization method is recommended because of its greater accuracy. The Green-

Gauss Cell Based gradient spatial discretization method is adequate if the mesh is evenly

spaced in the system current direction, and if there are not large differences in the electrical

conductivities in the materials used in the simulation.

Note

In transient simulations, you should start the calculation with a smaller time step ( ~

Note

seconds) initially. The time step can be increased to a large value (for example,  seconds),

however, you will likely need to search for a suitable value to make sure reasonable conver-

gence is achieved within each time step.

You can perform post-processing using standard ANSYS Fluent quantities and by using user-defined

scalars and user-defined memory allocations. When using the Battery model, the following additional

variables will be available for postprocessing:

Under User-Defined Scalars...

– Electric Potential

– Diff Coef of Electric Potential (the electrical conductivity of the conductive field)

Under User-Defined Memory...

– Interface Current Density (the separator current density, that is J (A/m2))

– X Current Density

– Y Current Density

– Z Current Density

– Magnitude of Current Density

– Volumetric Ohmic Source (the energy source due to the electric Joule heating)

– Electrochemistry Source

– Activation Over-Potential (the net electrode potential change across the anode and cathode of the

system when there is a current flowing through the system, that is,

(Volts)

– Depth of Discharge

– U Function

– Y Function

– Separator Voltage Jump (the net potential difference across the separator)

– Effective Electric Resistance (the effective resistance of the separator used in the potential field calcu-

lation)

– Other

By default, the ANSYS Fluent Battery Model defines several user-defined scalars and user-defined

lation)

– Other

memory allocations, described in Table . : User-Defined Scalar Allocations (p. ) and Table . : User-

Defined Memory Allocations (p. ).

Table . : User-Defined Scalar Allocations

Electric Potential (Volts)

UDS

Diff Coef of Electric Potential

UDS

Table . : User-Defined Memory Allocations

Interface Current Density

UDM

X Current Density

UDM

Y Current Density

UDM

Z Current Density

UDM

Magnitude of Current Density

UDM

Volumetric Ohmic Source

UDM

Electrochemistry Source

UDM

Activation Over-Potential

UDM

Depth of Discharge

UDM

U Function

UDM

Y Function

UDM

Separator Voltage Jump

UDM

Effective Electric Resistance

UDM

Other

UDM

Note

For field variables that are stored in UDM, use the corresponding variables for post pro-

cessing. Post processing the UDM itself is not recommended.

For reviewing simulation results in CFD Post for cases involving UDM or UDS, export the

solution data as CFD-Post-compatible file (.cdat) in Fluent and then load this file into

CFD-Post.

You can incorporate your own formulations and data for the properties of the battery using the

batt_user.c source code file.

The following listing represents a description of the contents of the batt_user.c source code file:

real CONDUCTIVITY_CELL(cell_t c, Thread *t): Returns values for the electrical conductivity

for cells inside conductive zones, overwriting the values set in the Electric Field tab of the Battery Model

real CONTACT_RESIST_FACE(cell_t f, Thread *t): Returns values for the electrical contact

resistance, overwriting the values set in the Electric Field tab of the Battery Model dialog box.

real Compute_U (face_t f, Thread *t, real DOD, real dUdJ, real a[], real

dUdJ): Returns values for both U and the derivative of U with respect to J (dUdJ). Note that DOD represents

the depth of discharge and a[] is the set of U coefficients.

real Compute_Y (face_t f, Thread *t, real DOD, real b[]): Returns values for Y.

Note that DOD represents the depth of discharge and b[] is the set of Y coefficients.

.... Compiling the Customized Battery Source Code

This section includes instructions on how to compile a customized Battery user-defined module. Note

that you can also refer to the file INSTRUCTIONS-CLIENT that comes with your distribution (see

addons/battery).

Important

It is assumed that you have a basic familiarity with compiling user-defined functions (UDFs).

For an introduction on how to compile UDFs, refer to the Fluent Customization Manual.

You will first want to use a local copy of the battery directory in the addons directory before you

recompile the Battery module.

..... Compiling the Customized Source Code Under Linux

. Make a local copy of the battery directory. Do not create a symbolic link.

Important

The custom version of the library must be named according to the convention used

by ANSYS Fluent: for example, battery.

. Change directories to the battery/src directory.

. Make changes to the batt_user.c file.

. Edit the makefile_slave.nt located in the src/ directory and make sure that the FLUENT_INC

variable correctly refers to the current ANSYS Fluent installation directory. Be careful not to leave any

trailing spaces when you make your changes.

. Define the FLUENT_ADDONS environment variable to correspond to your customized version of the

Battery module.

. Change directories to the battery/ directory.

. Issue the following make command:

make FLUENT_INC=[ansys_inc/v195/fluent] FLUENT_ARCH=[arch]

f Makefile-client

where your_arch is lnx86 on LINUX, or ultra on the Sun operating system, etc.

The following example demonstrates the steps required to set up and run a customized version of

the Battery module that is located in a folder called home/sample:

Make a directory (for example, mkdir -p /home/sample).

Copy the default addon library to this location.

cp -RH [ansys_inc/v195/fluent]/fluent19../addons/battery

/home/sample/battery

Using a text editor, make the appropriate changes to the batt_user.c file located in

/home/sample/battery/src/batt_user.c

Edit the makefile_slave.nt located in the src/ directory and make sure that the FLUENT_INC

Build the library.

cd /home/sample/battery

Set the FLUENT_ADDONS environment variable (using CSH, other shells will differ).

setenv FLUENT_ADDONS /home/sample

Start ANSYS Fluent and load the customized module using the text interface command.

..... Compiling the Customized Source Code Under Windows

. Open Visual Studio.NET at the DOS prompt.

. Make sure that the FLUENT_INC environment variable is correctly set to the current ANSYS Fluent in-

stallation directory (for example, ANSYS Inc\v195\fluent).

. Make a local copy of the battery folder. Do not create a shortcut.

. Enter the battery\src folder.

. Return to the battery folder.

. Issue the following command in the command window:

nmake /f makefile_master-client.nt

This section describes how to use the MSMD and Cell Network modeling capability in ANSYS Fluent.

Only the procedural steps related to battery modeling are shown here. For information about inputs

related to other models used in conjunction with the battery model, see the appropriate sections for

those models in the ANSYS Fluent Fluent User's Guide (p. ). For more details on the modeling approach,

refer to Dual-Potential MSMD and Circuit Network Battery Models.

Information about using the model is presented in the following sections:

... Geometry Definition

... Loading the Dual-Potential MSMD Battery Module

... Setting up the Dual-Potential MSMD Battery Model

... Using Parameter Estimation Tools

... Initializing the Battery Model

... Modifying Material Properties

... Solution Controls for the Dual-Potential MSMD Battery Model

... Postprocessing the Dual-Potential MSMD Battery Model

Note the following limitations when using the Dual-Potential MSMD Battery model:

For battery pack simulations, all batteries in the pack must be identical initially, having the same battery

type with the same initial conditions.

For battery pack simulations, all batteries in the pack must have the nPmS connection pattern; that is, n

batteries connected in parallel, and then m such units connected in series.

A conductive zone must be continuous. Disconnected zones cannot be grouped as one entity.

System positive and negative tabs must be continuous surfaces. Disconnected faces cannot be grouped

together as one entity.

The positive and negative tabs must be connected by either the real tab/busbar conductive volumes or

the virtual connections defined through a file.

A battery tab cannot be directly contact another battery tab.They must be connected by busbars.

In the MSMD and Cell Network frameworks, the negative and positive current collectors, anode, and

cathode are not resolved, and the battery is regarded as a homogeneous body. The computational

mesh does not have to be adjusted to all layers present in the battery domain. The following zones

have to be identified when creating the battery mesh:

Cell

Tab

Busbar (for battery pack cases with real battery connections)

When using the real battery connections you need to create busbar zones and specify them under

Cell

Tab

Basbar Components (see Specifying Conductive Zones (p. ) for details). Since both tab zones and

busbar zones are passive zones, you can group them all under busbar for simplicity. However, busbars

sometimes may not be assigned to the tab zone category because a battery tab zone cannot directly

connect to another battery tab zone.

When using the virtual battery connections you do not need to create busbar zones. You only need

to create tab zones (if you have tab volumes) and specify them under Tab Components (see Specifying

Conductive Zones (p. ) for details).

. none

. MHD Model

Select the dual-potential MSMD battery model by entering the module number . During the loading

process, a Scheme library containing the graphical and text user interface, and a UDF library containing

a set of user-defined functions (UDFs) for the battery module are loaded into ANSYS Fluent. This is

reported to the console. The UDF library also becomes visible as a new entry in the UDF Library

Manager dialog box. The basic setup of the battery model is performed automatically when the battery

module is successfully loaded.

Using the Dual-Potential MSMD and Cell Network Battery Models

Once the module has been loaded, you can enable the Dual-Potential MSMD Battery Model, set battery

model parameters and assign properties to the relevant regions in your battery.

To enable the MSMD battery model: In the Outline View under the Models branch, right-click MSMD

Battery Model and click Edit... in the menu that opens.

Setup → Models → MSMD Battery Model

Edit...

Figure . : The MSMD Battery Model Option in the Outline View

In the MSMD Battery Model dialog box that opens, select the Enable Battery Model check box to

activate the model.

The MSMD Battery Model dialog box expands to reveal additional model options and solution controls.

The inputs for the battery model are entered using the following tabs:

Model Options

contains the general model settings to define problems using the battery model.

Model Parameters

is where you specify the parameters to be used for solving the model equations.

Conductive Zones

allows you to select zones for the active, tab and busbar components.

Electric Contacts

allows you to define the contact surface and external connectors.

Advanced Option

allows you to qukckly check the selected electrochemical submodel behavior using the Echem model in

a standalone mode, and also enable a thermal abuse model and specify its parameters.

Note

Note

When setting up the model, you can click the Apply button to save your input values and

your choices for your model. To restore the last saved settings for all tabs, click the Reset

button.

.... Specifying Battery Model Options

.... Specifying Battery Model Parameters

.... Specifying Conductive Zones

.... Specifying Electric Contacts

.... Specifying Advanced Option

.... Specifying External and Internal Short-Circuit Resistances

In the Model Options tab, you can select the electrochemical battery submodel and set various

model options, solution controls, and electrical parameters.

Figure . : The MSMD Battery Model Dialog Box (Model Options Tab)

The following submodels are available in ANSYS Fluent under the E-Chemistry Models group box:

NTGK Empirical Model

is an empirical model.This is the simplest and the least expensive model. It also requires the fewest

model inputs.The model uses the same NTGK method as that used by the Single-Potential Empirical

model. However, in this case, it solves two potential equations continuously instead of one potential

equation with a jump condition at the separator over all conductive zones.The model cannot accurately

capture the battery's dynamic (inertial) response.

Equivalent Circuit Model

is a semi-empirical model. It has limited capability for predicting the battery dynamic behavior.

Newman P2D Model

is the most comprehensive physics-based battery model. It is computationally expensive, and it requires

extensive user input of battery-related fundamental information.

User-defined E-Model

is the user-specified electrochemical submodel.To be able to use this option in the Fluent MSMD

method framework, you must provide the void user_defined_echem_model() function in the

customizable cae_user.c source code file.

For Solution Method for E-Field, if you select:

Circuit Network Method, none or one potential equation will be solved, depending on whether Joule

heating in passive zones is included or not. See Circuit Network Solution Method in the Fluent Theory

Guide for more information about this method.

Solving Transport Equation, two potential equations will be solved during each iteration in the simulation.

Reduced Order Method, the solution will be obtained (faster) using the reduced order method (ROM).

You can use this option if the two conditions listed in Reduced Order Solution Method (ROM) are met.

Note that, prior to using the ROM, you must first run a simulation with the Solving Transport

Equation option for at least three time steps. ANSYS Fluent will use these results as reference po-

tential fields for the ROM method.

Once you have selected Reduced Order Method, you can set Number of Sub-Steps/Time Step.

Using this value, you can specify the ratio of the time steps for thermal and electro-chemistry cal-

culations. For example, if the Number of Sub-Stepes/Time Step is set to , the solver will use

one tenth of the CFD time step for the electro-chemistry calculation.

Important

Important

If internal short circuit occurs in a battery, the Reduced Order Method cannot be used.

For Energy Source Options, you can:

Enable Joule Heat in Tab/Busbar Zones (default) in order to include the Joule heating source in the

thermal energy Equation . in the battery passive conducting zones, including tabs and busbars,

Enable Joule Heat in Active Zones  (default) in order to include the Joule Heating source in the thermal

energy equation Equation ..

Enable E-Chem Heat Source (default) in order to include the heat source due to electrochemistry in the

thermal energy equation Equation ..

For Solution Controls, you can:

Set Current Under-Relaxation Factor.The volumetric current density used in the two potential equations

are under-relaxed according to this factor.The default value of . may be sufficient for most cases.The

values in the range of .–. are recommended.

Set Voltage Correction Under-Relaxation Factor.The default value of . is acceptable for most cases.

You should reduce this value only if the convergence difficulty occurs during the solution of the potential

(Equivalent Circuit Model and Newman P2D Model) Select the Cluster Cells check box to enable cell

clustering and specify the number of clusters Nx , Ny , and Nz  in X,Y, and Z directions respectively.The

solver will divide the battery domain into Nx  x Ny  x Nz  clusters and solve submodel equations for each

cluster using cluster-average information.The default values for Nx , Ny , and Nz  are , , and , respectively.

For the initial run, the default settings are recommended.This option is available only for the Solving

Transport Equation and Reduced Order Method solution methods.

For Electrical Parameters, you can specify the following operation conditions:

Set the Nominal Cell Capacity (the capacity of the battery cell).

For the Solution Options, if you select:

– Specified C-Rate, you can set a value for the following:

→ Discharge C-Rate (the hourly rate at which a battery is discharged; a positive value means dis-

charging C-rate and a negative value means charging C-rate). In this case, the total current at

the cathode tabs is fixed as the product of C-Rate and Nominal Capacity, while the electrical

potential is anchored at zero on the anode tabs.

→ Min. Stop Voltage and Max. Stop Voltage.The simulation will automatically stop once the

battery cell voltage reaches the minimum or maximum value. For a battery pack, the battery-

average cell voltage is used.

– Specified System Current, you can set the following:

→ System Current (applied at the cathode tabs). A positive value means discharging current and

a negative value means charging current.

→ Min. Stop Voltage and Max. Stop Voltage. (Same as for Specified C-rate.)

– Specified System Voltage, you can set a value for the System Voltage (applied to the cathode

tab; the anode tab has a voltage of  V).

– Specified System Power, you can specify the following:

→ System Power. If you specify the total power output from your battery, Fluent solver will ensure

that the product of the system current and voltage equals the system power. A positive value

means discharging power output and a negative value means charging power input.

– Specified Resistance, you can specify the external electric resistance in an external short-circuit

→ External Resistance. If you specify the external electric resistance in Ohm, the Fluent solver will

ensure that the ratio of the system voltage to the system current equals the specified external

resistance.

– Set in Boundary Conditions, you can set the UDS boundary conditions directly, for example, the

voltage value or the current value (specified flux), using the Boundary Conditions task page in

ANSYS Fluent for the specific face zone.

– Using Profile, you can select Time-Scheduled or Event-Scheduled under Profile Type and

provide time-dependent or event-dependent input (respectively) for the C-rate, current, voltage,

or power.The time-scheduled and event-scheduled profiles enable you to change the electric load

type and electric value in the simulation on the fly.

Once the profile type is selected, you can browse to the ASCII text file with either the .dat

or .txt file extension that you generated beforehand.

The inputs for the Time-Scheduled and Event-Scheduled profiles are described below.

→ The Time-Scheduled profile file must be organized in three columns:

. Time

. Electric load value

. Electric load type

The electric load type is defined by an integer number:

: C-rate

: Current

: Voltage

: Power

: External electric resistance

. Time

: C-rate

: Current

: Voltage

: Power

For example, the below time-scheduled profile:

.

. -

specifies the following battery charging scenario:

. The battery is discharged at  A for the first  seconds.

. The battery discharge continues at  W for the next  seconds.

. The battery is charged at a constant  C-rate for the last  seconds.

Note

For current, power, or C-rate, a positive value means discharging and a negative

value means charging.

The unit of the variables in the input file is always SI.

ANSYS Fluent solver uses linear interpolation of your time-scheduled profile data in the

problem simulation. If you want to capture a sudden change in the profile accurately, use

smaller time gaps to describe the profile.

→ The Event-Scheduled profile file must be organized in the following five columns:

Just as in the time-scheduled profile, the electric load type is defined by an integer

number:

: C-rate

: Current

: Voltage

: Power

. Forwarding condition

The forwarding condition (FC) is defined by an integer number:

: Time > FC_Value

: I < FC_Value (discharging current minimum)

: I > FC_Value (charging current maximum)

: V < FC_Value (system voltage minimum)

: V > FC_Value (system voltage maximum)

: P < FC_Value (discharging power minimum)

: P > FC_Value (charging power maximum)

. Forwarding condition value

. Stop flag

The stop flag is an integer value of  or , where  specifies that the run should con-

. Stop flag

tinue to the next event entry line, and  specifies that the run should end.

For example, the below event-scheduled profile:

.

.

. -

specifies the following scenario:

. The battery is discharged at  C rate until the voltage reaches . V.

. The battery is charged at constant current  A until the voltage reaches . V.

. The battery keeps charging at . V until the current is greater - A.The simulation stops

after reaching this point.

Note

Any time-scheduled profile can be rewritten in an event-scheduled profile format, but

not vice-versa. The example shown in the time-scheduled profile can be redefined in an

event-scheduled profile format as follows.

Both profile types can be read into ANSYS Fluent. You can choose the most convenient

one to use in your specific application.

The Model Parameters tab of the MSMD Battery Model dialog box allows you to specify the sub-

model-specific parameters to be used for solving the submodel equations. The Model Parameters

tab contains only the entry fields for parameters related to the electrochemical submodel you have

chosen in the Model Option tab. A detailed description of inputs for each submodel is given in the

sections that follow.

..... Inputs for the NTGK Empirical Model

..... Inputs for the Equivalent Circuit Model

..... Inputs for the Newman’s P2D Model

..... Input for the User-Defined E-Model

Figure . : Model Parameters Tab—NTGK Model

For the NTGK Empirical Model, you can define the model parameters used in Equation . using

the following Data Types:

Polynomial

When using the Polynomial data type, you can directly specify polynomial coefficients for

,

,

and temperature correction in Equation ..

Table

When using the Table data type, you can define a 2D lookup table for each NTGK model parameter.

Tabular data are entered in the corresponding parameter data table dialog box that opens by

clicking the relevant button in the NTGK parameter data table group box (see Figure . : NTGK

U-parameter Data Table Dialog Box (p. )).

Figure . : NTGK U-parameter Data Table Dialog Box

For each NTGK model parameter, you can specify up to  DOD levels and temperature levels.

For each DOD-temperature pair, you must enter the corresponding model parameter value. Each

table can be exported to or imported from a file by clicking Write or Read, respectively, in the

parameter data table dialog box.

Note

The model parameters for the NTGK Model Polarization Parameters are based on battery

cell polarization test curves. Obtaining model parameters (other than the default values) can

be dependant on your battery configuration and material properties.The default values are

taken from Kim’s paper . If you model a battery having a different design, you must provide

a different set of battery parameters.

ANSYS Fluent provides the parameter estimation tool for computing

and  functions from

the battery's testing data—constant discharging curves.The tool is available via the text-user-

interface (TUI). For details, see Using Parameter Estimation Tools (p. ).

You can also set values for Initial DoD and Reference Capacity (

in Equation . ). The default

value of  for Initial DoD indicates the fully-charged state of the battery cell. Reference Capacity

is the capacity of the battery that is used in experiments to obtain the

and

model parameters.

Nominal and reference capacities may have different values.

Figure . : Model Parameters Tab—Equivalent Circuit Model

For the Equivalent Circuit Model, you can define resistors' resistances (Rs, R1, and R2), capacitors'

capacitances (C1 and C2), and the open circuit voltage (Voc) using the following Data Types:

Chen's original

For the Chen's original data type, you need to specify all coefficients in Equation ..

For the Polynomial data type, you can directly specify polynomial coefficients in Equation ..

Table

For the Table data type, you can define a 2D lookup table for each ECM parameter. See Inputs

for the NTGK Empirical Model (p. ) for more information on how to define model parameters

in a table data type.

In addition, you can turn on the Using different coefficient for charging and discharging option

and specify the coefficients for Charging parameters.

You can also set values for Initial State of Charge and Reference Capacity (

The default value of  for Initial State of Charge indicates the fully-charged state of the battery

cell. Reference Capacity is the capacity of the battery that is used in experiments to obtain the

model parameters. Note that nominal and reference capacities may have different values.

Note

The values of model parameters for the Equivalent Circuit Model are battery specific and

need to be specified before conducting a simulation.The default values are taken from Chen

. If you model a battery of different design, you should specify a different set of battery

ANSYS Fluent provides the parameter estimation tool for computing the ECM parameters

from the battery's testing data—typically, the HPPC data.The tool is available via the text-

user-interface (TUI). For details, see Using Parameter Estimation Tools (p. ).

Figure . : Model Parameters Tab—Newman’s P2D Model

The following parameters are available under Model Parameters for the Newman’s P2D model:

Thickness

are ,

, and  in Equation ..

Number of Grids

is a number of grid points used to discretize the positive electrode, negative electrode, and separator

zones.

Grid Size Ratio

is used to create a biased mesh.The default value of  corresponds to a uniform mesh.

Particle Diameter

is the particle diameter of the active material.

Number of Grids in Solid

is the number of grid points used to discretize the sphere of particles.

Grid Size Ratio in Solid

is used to create a biased mesh for the solid phase.The default value of  corresponds to a uniform

mesh.

Max. Solid Li+ Conc

is the maximum concentration of Lithium in the solid phase (used in Equation . ).

Stoi. at % SOC

is the stoichiometry at % SOC that is used to compute theoretical capacity and initial lithium concen-

tration in the electrode.

is the stoichiometry at % SOC that is used to compute theoretical capacity and initial lithium con-

centration in the electrode.

Init. Solid Li+Conc.

is the initial lithium concentration in the electrode.

Init. Electrolyte Li+Conc.

is the initial lithium concentration in the electrolyte phase.

Volume Fraction of Electrolyte

is the volume fraction of the electrolyte material in the electrode,

Filler Fraction

is the volume fraction of the filler material in the electrode,

Ref. Diffusivity

is the diffusion coefficient of lithium ion in the electrode at reference temperature

=°C,

in

Equation ..

Activation Energy E_d

is

Bruggeman Tortuosity exponent

is the Bruggeman tortuosity exponent,

Conductivity

is the electric conductivity,

Ref. Rate Constant

is the rate constant at reference temperature

=°C,

Activation Energy E_r

is

Trans. Coef. a

is the charge transfer coefficient at anode,

Trans Coef. c

is

is the charge transfer coefficient at cathode,

Electrolyte Diffusivity

is the diffusion coefficient of Li+ in the electrolyte phase,

t+ Factor

is the transference number of lithium ion,

You can also set values for Initial State of Charge. The default value of  for Initial State of Charge

indicates the fully-charged state of the battery cell.

Theoretical Capacity is computed from the Newman input parameters automatically and reported

in the MSMD Battery Model dialog box.

By default, ANSYS Fluent discretizes the lithium conservation equation and solves it numerically.

ANSYS Fluent also offers an option to use the reduced order method to solve the lithium diffusion

equation in solid . To use this method, select the Use Analytical Cs check box and enter the value

for the Cs Function Order.

Note

Model parameters are battery specific. The default values are taken from Cai & White .

To simulate a battery of different design, you should provide a user-specified set of battery

Figure . : Model Parameters Tab—User-Defined E-Model

The following parameters are available under User-Defined E-Chem Model Parameters:

Number of memories per cell

is the number of submodel parameters that need to be saved per computational cell during a simulation.

Initial SOC

is the value of the battery initial state of charge.

Reference Capacity

is the battery capacity (Ah).

The Conductive Zones tab of the MSMD Battery Model dialog box allows you to specify the active,

tab, and busbar zones.

Figure . : The MSMD Battery Model Dialog Box (Conductive Zones Tab)

In the Conductive Zones tab, select the appropriate zones for the Active Components, Tab Com-

ponents, and, if you simulate the battery pack with the real battery connections, the Basbar Com-

ponents. If you simulate the battery pack with the virtual battery connections, do not select any

zones under Basbar Components.

Battery cells are modeled as active zones; and battery tabs and busbars are modeled as passive zones.

Electrochemical reactions occur only in the active zones. The potential field is solved in both active

and passive zones.

The Electric Contacts tab of the MSMD Battery Model dialog box allows you to set the properties

of the Contact Surfaces and the External Connectors.

Figure . : The MSMD Battery Model Dialog Box (Electric Contacts Tab)

If you want to consider contact resistance, select zones for the Contact Surfaces and set the Contact

Resistance for any selected contact surface.

When using real connections, define the system negative and positive tabs under External Connectors.

When using the virtual connection option in a battery pack simulation, select the Use virtual battery

connection check box and in the Specify connection file text-entry box that appears, enter the file-

name containing the virtual connection definition.

The format for the connection definition file is as follows:

mP

nS

tab_N_1 tab_P_1

tab_N_2 tab_P_2

tab_N_3 tab_P_3

tab_N_4 tab_P_4

where:

The first line specifies the number of parallel batteries in a stage (mP).

The second line specifies the number of stages in series in a pack (nS).

The remaining lines contain pairs of the face names of the negative and positive tabs for each battery.

The battery data are listed in the following order: 1P1S ... 1PnS to mP1S ... mPnS.

For the above battery connection file example, the battery solver establishes the 1P4S connection

pattern.

The following figure shows the different resulting connection patterns for the different connection

data.

Once all conductive zones and the positive and negative tabs have been defined, ANSYS Fluent

automatically detects the battery network connection.

After you have defined all the conductive zones or modified zone related data, click Print Battery

System Connection Information, and review the battery connection information printed in the ANSYS

Fluent console window for any errors. If necessary, re-define the connections in the Conductive Zones

and Electric Contacts tabs.

Note

In the default battery solver configuration, the largest battery pack the solver can simulate

is 10P50S ( series stages with  parallel connected batteries per stage). However, you

can increase this limit to simulate larger battery packs using the following Scheme com-

mands:

(rpsetvar 'battery/max-n-parallel-per-stage m)

(rpsetvar 'battery/max-n-series n)

mands:

where m and n are the numbers of maximum parallel and series connections in the battery

pack, respectively.

Using the Advanced Option tab of the MSMD Battery Model dialog box, you can:

Check the selected electrochemical model behavior before running the CFD case by performing a quick

simulation of the electrochemical model in a standalone mode

Enable the Thermal Abuse Model, select the thermal abuse kinetics model, and define the corresponding

model parameters

Figure . : The MSMD Battery Model Dialog Box (Advanced Option Tab)

Running the Standalone Echem Model

Prior to running a coupled electrochemical-thermal simulation, you should perform a quick analysis

of your electrochemical model by simulating it in a standalone mode. The standalone model calculation

uses the operating conditions that you have specified in the Model Option tab (such as electric load

type and value) and the echem model parameters that you have defined in the Model Parameters

tab. This preliminary analysis will allow you to confirm the electrochemical behavior of the selected

submodel and, if necessary, adjust the model settings.

To run the echem model in a standalone mode:

. Click Run Echem Model Standalone.

. In the Standalone Echem Model dialog box that opens, specify the following parameters:

Report Time Step:The time interval at which the results will be saved and reported

Total Run Time:The total time for running the stand-alone model simulation

Reference Temperature:The temperature level at which you want to simulate your electrochemical

model

model

. Initiate the electrochemical model simulation by clicking Draw Profile.

Once the calculation is complete, the Plot Profile Data dialog box opens.

. Using the Plot Profile Data dialog box, visualize and analyze the results of the standalone echem model

simulation. Different profiles are available for different electrochemical models.

For the NTGK model, a time history profile, called ntgk-time-history-profile, is generated after the

calculation is complete.You can draw the X-Y plots of the following variables as a function of time:

– soc: the battery state of charge (SOC)

– voltage: the battery voltage

– current: the battery electric current

– power: the battery power output

For the ECM model, a time history profile, called ecm-time-history-profile, will be generated. In addition

to the variables available for the NTGK model, you can also draw the X-Y plots of the following variables

as a function of time:

– v1:

– v2:

For the Newman P2D model, the following two profiles will be generated:

– Time history profile p2d-time-history-profile

– Spatial field profile called p2d-field-profile

For the p2d-time-history-profile profile, you can plot the time history profile for the following

variables:

– current (see above)

– voltage (see above)

– power (see above)

– ce_x=

– ce_x=lp

– ce_x=lps

– ce_x=lpsn

– cs_x=

– cs_x=lp

– cs_x=lps

– cs_x=lpsn

– phis_x=

– phis_x=lp

– phis_x=lps

– phis_x=lpsn

– phie_x=

– phie_x=lp

– phie_x=lps

– phie_x=lpsn

where

– ce_x=lp

– ce_x=lps

– cs_x=

– cs_x=lp

– cs_x=lps

– phis_x=

– phie_x=

where

ce is the lithium-ion concentration in electrolyte phase at different locations

x= denotes the location of the outside face of the positive electrode

x=lp denotes the interface of the positive electrode and separator

x=lps denotes the interface between the separator and negative-electrode

x=lpsn denotes the outside face of the negative electrode

cs is the lithium concentration at the surface of the active material in electrode at

different locations

phis is the electric potential in the electrode solid phase at different locations

phie is the electric potential in the electrolyte liquid phase at different locations

For the p2d-time-history-profile profile, you can plot the spatial profiles of the following

variables at the end of the simulation:

– phi_e: the electric potential in electrolyte phase

– phi_s: the electric potential in electrode phase

– ce: the lithium-ion concentration in electrolyte phase

– cs_center: the lithium concentration in the center of the active electrode particles

– cs_average: the average lithium concentration in the active electrode particles

– cs_surf: the lithium concentration at the surface of the active electrode particles

Note

SI units are always used for all the variables in the X-Y plot.

Using the Thermal Abuse model

When you select One-equation kinetics model, you can specify the battery constants ,

,

,

,

and  used in Equation . through Equation ., as well as the initial value for .

When you select Four-equation kinetics model, you can specify the battery constants ,

,

,

,

and

,

,

,

,

,

,

and

used in Equation .) through Equation ., as well as the initial values for

,

,

, and

.

For both models, you can select Run thermal abuse model only (battery model is turned off) if

you want to solve the energy equation (Equation .) alone. Otherwise, the two battery potential

equations (Equation .) will also be solved.

Note

The kinetics parameters in thermal abuse models are specific to the battery material.The default

settings may not be appropriate for your battery.You must provide parameter data for your

own battery.

For the One-Equation thermal abuse model, you can use the ANSYS Fluent parameter estimation

tool available through the TUI to compute the kinetics parameters from the battery oven

testing data.The entry fields in the MSMD Battery Model dialog box will be automatically

populated with fitted results for the kinetics parameters. For details, see Using Parameter Es-

timation Tools (p. ).

The thermal abuse model is available only for the Solving Transport Equation solution

method.

For more information, see Thermal Abuse Model.

External Short-Circuit

To define the external short-circuit: In the MSMD Battery Model dialog box, under the Model Options

tab, select Specified Resistance and specify a value for External Resistance. See Specifying Battery

Model Options (p. ) for details.

Internal Short-Circuit

The intensity of the internal short-circuit is determined by the value of volumetric contact resistance

(External and Internal Electric Short-Circuit Treatment. In the ANSYS Fluent battery model, this

value is saved in a predefined user-defined memory allocation, Short Circuit Resistance. You can

modify the value of this user-defined memory allocation to simulate the internal short circuit.

By default, the contact resistance is set to a very large number, so that

and

, that is,

there is no internal short.

You can simulate an internal short-circuit using either of the following two ways:

Patching: Patch the contact resistance to the short circuit zone.The short circuit zone can be defined by

creating a region cell register using the Region Register dialog box. See Region in the Fluent User's

Guide (p. ) for more details.

Using UDF: Use DEFINE_ADJUST or DEFINE_ON_DEMAND UDFs to specify the contact resistance

using the UDM macro, C_UDMI(c,t,SHORT_R).The contact resistance could be a function of location

and time. See the Fluent Customization Manual for details.

The internal short-circuit model is available only for the Solving Transport Equation solution method.

The parameters for the NTGK, ECM, and one-equation thermal abuse models are battery specific. In

theory, they can be fitted from some standard battery's testing data. ANSYS Fluent provides parameter

estimation tools for computing parameters for these models.

The parameter estimation tool can be accessed through the text-user-interface (TUI):

define/models/battery-model/parameter-estimation-tool

Parameter Estimation for Model:

: NTGK Model

: ECM Model

: ECM Model

: Thermal Abuse Model

Model option:  []

After you select a model option, you will be prompted for information specific to the selected model.

Using the parameter estimation tool for the NTGK model

The NTGK model parameters are fitted as functions of DOD and temperature. To fit the NTGK model

parameters, you need to have battery's discharging curves at different constant C-rates. You can use

testing data at different temperatures.

To use the parameter estimation tool for the NTGK model:

. At the prompt, specify Number of temperature levels and Number of discharging

curves per temperature level.

. For each temperature level, enter the temperature value and provide files containing testing data at the

specified temperature.

Note

The input file order does not matter.

For each C-rate, you must provide a separate file in text format. At least two input files with data

at different C-rates are required to get meaningful fitting results.

The file format will be displayed in the Fluent console. An example of an input file is shown below.

Crate .

.0000e+   .1097e+

.0000e+   .1094e+

.0000e+   .1092e+

...

.6000e+   .1010e+

...

The first line of the file starts with Crate followed by a C-rate value separated by a space. The

lines that follow contain pairs of space-separated time-voltage values.

. After you specify input file names for different C-rate testing data, enter responses to the following

prompts:

Battery capacity: Specifies capacity of the tested battery. Its value will be automatically transferred

and displayed in the Reference Capacity text entry box in the MSMD Battery Model dialog box

(Model Parameters tab).

Number of DOD-levels: Is used in the fitting.The default value of  DOD levels is usually sufficient.

If you provide testing data files at different temperatures, the parameter estimation tool will perform

the fitting for each temperature level. ANSYS Fluent will report the fitted results in the console and

automatically pass them in a table data type to the parameter data table dialog boxes. The Table data

type will be automatically selected in the MSMD Battery Model dialog box (Model Parameters tab).

This will allow you to consider the temperature-dependent effect.

If you use testing data from only one temperature level, the fitting results in both polynomial and

table data types will be transferred to the MSMD Battery Model dialog box and to the parameter

data table dialog boxes. In this case, the Polynomial data type will be automatically selected in the

MSMD Battery Model dialog box, respectively. You can use either data type in your simulation.

The following is an example of using the parameter estimation tool for fitting the NTGK model para-

meters:

/define/models/battery-model> parameter-estimation-tool

: ECM Model

Number of temperature levels: []

Number of discharging curves per temperature level: []

-- Make sure every input file has this format --

Crate     .

time_1    voltage_1

time_2    voltage_2

...       ...

------------------------------------------------

Crate     .

...       ...

Temperature (K) []

file name for curve  [] ntgk-1C-300K.dat

file name for curve  [] ntgk-2C-300K.dat

file name for curve  [] ntgk-3C-300K.dat

file name for curve  [] ntgk-4C-300K.dat

file name for curve  [] ntgk-5C-300K.dat

file name for curve  [] ntgk-1C-290K.dat

file name for curve  [] ntgk-2C-290K.dat

file name for curve  [] ntgk-3C-290K.dat

file name for curve  [] ntgk-4C-290K.dat

file name for curve  [] ntgk-5C-290K.dat

file name for curve  [] ntgk-1C-310K.dat

file name for curve  [] ntgk-2C-310K.dat

file name for curve  [] ntgk-3C-310K.dat

file name for curve  [] ntgk-4C-310K.dat

file name for curve  [] ntgk-5C-310K.dat

Battery capacity (Ah) [.]

Number of DOD-levels []

To help you assess and debug the fitting process, after running the fitting tool, ANSYS Fluent automat-

ically creates a folder called fittingresult in your working directory. In this folder, Fluent stores

the following automatically generated files:

ntgk-curve#-t#-crate#.dat: A fitting result text file with three columns of data (t, experimental

data, and fitting data) for each Crate curve.You can use this file in a third-party software for further

processing.

ntgk-curve#-t#-crate#.xy: An XY plot file that can be plotted in Fluent to examine the fitting

quality.

ntgk-generatepic.scm: A scheme file that can be run in Fluent to draw all the generated XY plots

and automatically save them as image files.

ntgk-t#-u-function.xy, ntgk-t#-y-function.xy, and ntgk-t#-intermediate.xy: XY

plots of fitted U,Y and V~I curves.

Using the parameter estimation tool for the ECM model

To fit the ECM model parameters, you need to have battery's Hybrid Pulse Power Characterization

(HPPC) testing data at different SOC levels. Similar to the NTGK model, you can use testing data at

different temperatures.

To use the parameter estimation tool for the ECM model:

. At the prompt, specify Number of temperature levels and Number of different SOC-

level curves per temperature level.

Note

For each SOC level, you must provide a separate file with battery's testing data points in text format.

At least one valid SOC level testing data is required per temperature level. For good simulation

results, the range of SOC levels used in the testing should cover the SOC range simulated in the

CFD runs.

SOC .

I   .

.0000e-    .2292e+

...

.1800e+    .1041e+

...

The first line of the file starts with SOC followed by a SOC value separated by a space. The second

line contains the pulse current information (I followed by a pulse current value). The remaining

lines contain pairs of space-separated time-voltage values. The input data must include data from

the rest period, the pulse period, and the relaxation period in the testing.

. After you specify input file names, enter responses to the following prompts:

Circuit Model:

– Enter  if you want to use the 4P parameter model (one RC loop circuit)

– Enter  if you want to use the 6P parameter model (two RC loop circuit).

Fitting Method:

– Enter  if you want to use the Jiang-Hu method

The Jiang-Hu method uses HPPC testing data only from the relaxation period.

– Enter  if you want to use the Levenberg-Marquardt method.

The Levenberg-Marquardt method uses data from both pulse and relaxation periods.

. Although the parameter estimation tool does not require the testing battery's capacity, you must specify

this value.

data table dialog boxes, respectively. In this case, the Polynomial data type will be automatically se-

lected in the MSMD Battery Model dialog box. You can use either data type in your simulation.

Note

Because the parameter estimation tool attempts to calculate six or four ECM model parameters

from a non-linear data regression process for each SOC curve, the testing data for each SOC

curve should be sufficiently large in order to obtain a good fitting.

The parameter estimation tool always fits the experimental data into either six parameters used

in the Chen's circuit shown in Figure . : Electric Circuits Used in the ECM Model or four para-

meters in the reduced Chen's circuit with only one RC loop.

To obtain optimal fitting of HPPC testing data, you can try different combinations of the circuit

model and the fitting method.The six-parameter circuit model has more physics, but the four-

parameter circuit model is generally more robust. As for the fitting method, the Levenberg-

Marquardt algorithm is in general more robust than the Jiang-Hu algorithm.You can start with

the six-parameter model, and then, if the fitting results are not satisfactory, switch to the four-

parameter model.

The following is an example of using the parameter estimation tool for fitting the ECM model paramet-

ers.

/define/models/battery-model> parameter-estimation

: ECM Model

Number of different SOC-level curves per temperature level: []

SOC       .

I         .

...       ...

SOC       .

I         .

...       ...

where SOC: soc level

I: pulse current

file name for curve  [] soc01-290K.dat

file name for curve  [] soc02-290K.dat

file name for curve  [] soc03-290K.dat

file name for curve  [] soc04-290K.dat

file name for curve  [] soc05-290K.dat

file name for curve  [] soc06-290K.dat

file name for curve  [] soc07-290K.dat

file name for curve  [] soc08-290K.dat

file name for curve  [] soc09-290K.dat

file name for curve  [] soc10-290K.dat

file name for curve  [] soc01-300K.dat

file name for curve  [] soc02-300K.dat

file name for curve  [] soc03-300K.dat

file name for curve  [] soc04-300K.dat

file name for curve  [] soc05-300K.dat

file name for curve  [] soc06-300K.dat

file name for curve  [] soc07-300K.dat

file name for curve  [] soc08-300K.dat

file name for curve  [] soc09-300K.dat

file name for curve  [] soc10-300K.dat

file name for curve  [] soc01-310K.dat

file name for curve  [] soc02-310K.dat

file name for curve  [] soc03-310K.dat

file name for curve  [] soc04-310K.dat

file name for curve  [] soc05-310K.dat

file name for curve  [] soc06-310K.dat

file name for curve  [] soc07-310K.dat

file name for curve  [] soc08-310K.dat

file name for curve  [] soc09-310K.dat

file name for curve  [] soc10-310K.dat

Battery capacity (Ah) [.] .

: 4P parameter model (one RC loop)

: 6P parameter model (two RC loops)

Circuit model option:  []

: Jiang-Hu Method (JH)

: Levenberg-Marquardt Method (LM)

Fitting method option:  []

ecm-curve#-t#-soc#.dat: A fitting result text file with three columns of data (t, experimental

data, and fitting data) for each curve.You can use this file in a third-party software for further pro-

cessing.

ecm-curve#-t#-soc#.xy: An XY plot file for each fitting curve.You can plot this file in Fluent and ex-

amine the fitting quality.

ecm-createpic.scm: A scheme file that can be run in Fluent to draw all the generated XY plots and

automatically save them as image files.

Using the parameter estimation tool for the thermal abuse model

Kinetics data used in the thermal abuse model are battery specific. Reaction kinetics parameters in

Equation . can be fitted by using testing data (for example, Oven test or ARC). Temperature vs.

time data collected from experiment for a battery cell under thermal abuse condition can be used as

input in the parameter estimation tool.

The following thermal balance equation is used to describe the heating process and in the kinetics

parameter fitting of the temperature-time data:

(.)

where:

= volume

= external area

= material density

= heat transfer coefficient

= surface emissivity

= heat of reaction

= pre-exponential factor

= activation energy

= reaction progress variable

= ambient temperature

= enclosure temperature for radiation

and  = reaction order parameters

The equation will be printed in the console for your reference.

You will be prompted to specify a file name for temperature testing data and values for the variables

used in Equation . (p. ).

After running the parameter estimation tool for the one-equation thermal abuse model, ANSYS Fluent

will obtain and pass the following parameter to the MSMD Battery Model dialog box (Advanced

Option tab): A, E, HW, m, and n. These parameters will also be printed in the console.

There are two ways to initialize the battery model:

Initialize the flow field from the Solution Initialization task page.The battery model will be initialized

also.

Initialize the battery model in isolation by clicking the Init button in the MSMD Battery Model dialog

box. Other flow variables remain untouched.

Use the second method if you want to freeze the flow field and use a different battery model

to simulate the battery field. When switching from one battery submodel to another, the battery

model must be re-initialized. The Init button in the MSMD Battery Model dialog box provides

a convenient way to accomplish this if you do not want to initialize the flow field.

When using the MSMD battery models in ANSYS Fluent, you must define the UDS diffusivity of the

cell, tab, and busbar materials.

.... Specifying UDS Diffusivity for the Active Material

The UDS diffusivity of the active material must be defined using the defined-per-uds method as

follows:

. In the Create/Edit Materials dialog box, select defined-per-uds from the drop-down list for UDS Dif-

fusivity.

The UDS Diffusion Coefficients dialog box is opened listing the uds- and uds- scalar diffusion

coefficients defined in ANSYS Fluent. Both scalars are set at the default values of 1e+.

. Modify the default values for uds- and uds- (if necessary).

. For anisotropic material, select the orthotropic, cyl-orthotropic, or anisotropic option from the Coef-

ficient drop-down list and specify the diffusion coefficients as described in Fluent Customization

Manual.

Note, that if the UDS Diffusion Coefficients are defined through the defined-per-uds option,

the Fluent solver does not use the value for Electrical Conductivity.

.... Specifying UDS Diffusivity for the Passive Material

The UDS diffusivity of the passive material must be defined using user-defined functions (UDF) as

follows:

. In the Create/Edit Materials dialog box, in the Properties group box, select user-defined from the

drop-down list for UDS Diffusivity.

. In the User-Defined Functions dialog box, hook the battery_e_cond::lib_caebat predefined

function provided by ANSYS Fluent. Note that this function cannot be modified.

. In the Create/Edit Materials dialog box, in the Properties group box, specify the value for Electrical

Conductivity (Fluent solver uses this value for the definition of battery_e_cond).

.... Defining Different Materials for Positive and Negative Electrodes

If electric conductivities

and

are different for the positive and negative electrodes, you must

define two different active materials, one for the odd zones and another for the even zones as follows:

. When defining a material for the odd zones, in the UDS Diffusion Coefficients dialog box, enter the

value of

for uds- and the value of

for uds-.

. When defining a material for the even zones, copy the odd-zone material that you have already defined

and modify the UDS0 and UDS1 scalars by interchanging their values, that is entering the value of

for

uds- and the value of

for uds-.

. In the Cell Zone Conditions task page, attach the odd zone material to the odd zones, and even zone

material to the even zones.To determine whether a zone belongs to the odd or even zone, use the Print

Battery System Connection Information button in the Electric Contacts tab of the MSMD Battery

Model dialog box and review the report printed in the console window.

When you use the battery models, two potential equations are solved in addition to other fluid dynamic

equations, depending on the type of simulation. The two potential equations (Potential Phi+ and

Potential Phi-) are listed in the Equations dialog box, where they can be enabled/disabled during

the solution process.

Solution →

Also, if required, define advanced settings the Advanced Solution Controls dialog box.

Setup →

Setup →

You can perform postprocessing using standard ANSYS Fluent quantities and by using user-defined

For the Circuit Network solution method with the Enable Joule Heat in Tab/Busbar Zones option:

– Under User-Defined Scalars...

→ Voltage Field

→ Diff Coef of Voltage Field

– Under User-Defined Memory...

→ Volumetic Ohmic Source  (the energy source due to the electric Joule heating in tab and busbar

zones)

For the Solving Transport Equation and Reduced Order Method:

→ Potential Phi+

→ Potential Phi-

→ Diff Coef of Potential Phi+

→ Diff Coef of Potential Phi-

→ Transfer Current Density

→ X Current Density

→ Y Current Density

→ Z Current Density

→ Magnitude of Current Density

→ Volumetric Ohmic Source (the energy source due to the electric Joule heating)

→ Total Heat Generation Source

→ Cell Voltage

→ Activation Over-Potential (the net electrode potential change across the anode and cathode of the

(Volts)

→ Depth of Discharge

→ U Function (the NTGK model only)

→ Y Function (the NTGK model only)

→ Volumetric Current Source (the transfer current density  in Equation ..

→ X Current Density for phi+

→ Y Current Density for phi+

→ Z Current Density for phi+

→ X Current Density for phi-

→ Y Current Density for phi-

→ Z Current Density for phi-

→ Short Circuit Resistance (internal short circuit intensity)

→ Volumetric Short Current Source (internal short current density)

→ Volumetric ECHEM Current Source (Total exchange current density)

→ Short-Circuit Heat Source (Joule heat due to internal short circuit)

→ Other

Note

solution data as CFD-Post-compatible file (.cdat) in Fluent and then load this file into CFD-

Post. This will ensure that the full variable set is available for post processing in CFD-Post.

You can incorporate your own correlations and data for the properties of the battery using the

cae_user.c source code file.

The following listing represents a description of the contents of the cae_user.c source code file:

real CONDUCTIVITY_CELL(cell_t c, Thread *t, int i): Returns values for the electrical

conductivity for cells inside passive conductive zones, overwriting the values set in the Create/Edit Mater-

ials dialog box.

resistance, overwriting the values set in the Electric Contacts tab of the MSMD Battery Model dialog box.

void Compute_ECM_VOC_and_CR(real soc, real T, int mode, real *Voc, real

RRs, real *RR1, real *RR2, real *CC1, real *CC2): Returns values for ECM model-related

parameters.You can use this function to implement ECM parameters in any function form.

real Compute_OCP_NE(real x, real T): Returns a value for open circuit potential at negative

electrode (

in Equation . ). By default, it is computed using functions in .

real Compute_OCP_PE(real x, real T): Returns a value for open circuit potential at positive

real Compute_kappa(real ce, real T): Returns a value for  (Equation . ). By default, it is

computed using functions in .

real Compute_Diff0_ce(real ce, real T): Returns a value for

(Equation . ). By default,

it is computed using functions in .

real Compute_tplus(real ce, real T): Returns a value for

(Equation . ). By default, it is

real Compute_Ds_PE(real cs, real T): Returns a value for the positive electrode diffusion

(Equation . ). By default, a constant value from GUI input is used.

real Compute_Ds_NE(real cs, real T): Returns a value for the negative electrode diffusion

real Compute_dlnfdlnce(real ce, real T): Returns a value for the term

from Equa-

tion .. By default, this term is not considered.

from Equa-

void Get_p2d_Postprocessing_Info(cell_t c, Thread *t, real T, real Vp,

real Vn): Exports detailed Newman's P2D model results.

real Compute_entropy_heat(real soc): Returns the entropic heat. By default, it is excluded in

all MSMD submodels, but can be included it by defining

in this UDF.

void user_defined_echem_model(int zero_start, int mode, real temperature,

real voltage, real current, real dtime, real *j_tmp, real *Qe_tmp, real

voltage_end): Defines the user-defined electrochemical model. A template for the user implementation

of the NTGK model is provided as an example.

This section includes instructions on how to compile a customized Battery user-defined module.

Important

For an introduction on how to compile UDFs, refer to the separate Fluent Customization

Manual.

You will first want to use a local copy of the msmdbatt directory in the addons directory before

you recompile the Battery module.

. Make a local copy of the msmdbatt directory. Do not create a symbolic link.

Important

by ANSYS Fluent: for example, msmdbatt.

. Change directories to the msmdbatt/src directory.

. Make changes to the cae_user.c file.

. Change directories to the msmdbatt/ directory.

make FLUENT_INC=[ansys_inc/v195/fluent/fluent19..] FLUENT_ARCH=[arch] -f Makefile-client

where arch is lnamd64 on LINUX.

. Make a directory (for example, mkdir -p /home/sample).

. Copy the default addon library to this location.

cp -RH [ansys_inc/v195/fluent]/fluent19../addons/msmdbatt

/home/sample/msmdbatt

. Using a text editor, make the appropriate changes to the cae_user.c file located in

/home/sample/msmdbatt/src/cae_user.c

. Build the library.

cd /home/sample/msmdbatt make FLUENT_INC=[ansys_inc/v195/fluent/fluent19..] FLUENT_ARCH=[arch]

. Set the FLUENT_ADDONS environment variable (using CSH, other shells will differ).

. Start ANSYS Fluent and load the customized module using the text interface command.

. Make a local copy of the msmdbatt folder. Do not create a shortcut.

a.

Create a directory for the custom msmdbatt libraries (for example, /home/custom-build).

b. Copy the msmdbatt library from the installation of ANSYS Fluent (Ansys Inc\v195\fluent\flu-

ent19..\addons) to your newly created directory.

stallation directory (for example, ANSYS Inc\v195\fluent\fluent19..).

. Enter the msmdbatt\src folder.

. Return to the msmdbatt folder.

nmake /f makefile_client.nt

MSMD Battery module in one of following ways:

Set the path to FLUENT_ADDONS globally.

In the Environment tab of Fluent Launcher, enter information for FLUENT_ADDONS in the Other

Environment Variables field, for example:

FLUENT_ADDONS=<driveletter>:\home\custom-build

Chapter : Modeling Fuel Cells

The ANSYS Fluent Fuel Cell Modules Chapter provides information about the background and the usage

of two separate add-on fuel cell modules for ANSYS Fluent. The available ANSYS Fluent add-on fuel cell

modules are:

PEMFC Model - allows you to model polymer electrolyte membrane fuel cells (PEMFC) with (or without)

micro-porous layers.This model is a new and recommended model for simulating energy conversion processes

in a PEM fuel cell. For more information, see PEMFC Model Theory.

Fuel Cell and Electrolysis Model - allows you to model polymer electrolyte membrane fuel cells (PEMFC),

solid oxide fuel cells (SOFC), and electrolysis with ANSYS Fluent.This model is sometimes referred to as the

Resolved Electrolyte model. Note that the PEMFC sub-model is being retained in the current release. However,

it will be removed in future releases because the new PEMFC Model mentioned above is more advanced

and complete as described in the Release Notes for ANSYS Fluent R17.. For more information, see Fuel Cell

and Electrolysis Model Theory.

SOFC With Unresolved Electrolyte Model - allows you to model solid oxide fuel cells (SOFC). For more inform-

ation, see SOFC Fuel Cell With Unresolved Electrolyte Model Theory.

Additional information about the model is provided in the following sections:

.. Using the PEMFC Model

.. Using the Fuel Cell and Electrolysis Model

.. Using the Solid Oxide Fuel Cell With Unresolved Electrolyte Model

The procedure for setting up and solving fuel cell problems using the PEMFC model is described in

detail in this chapter. Refer to the following sections for more information:

... Geometry Definition for the PEMFC Model

... Installing the PEMFC Model

... Loading the PEMFC Module

...Workflow for Using the PEMFC Module

... Setting Up the PEMFC Module

... PEMFC Model Boundary Conditions

... Solution Guidelines for the PEMFC Model

... Postprocessing the PEMFC Model

The ANSYS Fluent PEMFC model is composed of several user-defined functions (UDFs) and a graphical

user interface. The potential fields are solved as user-defined scalars. The capillary pressure, the water

content (water in dissolved phase), and liquid saturation in the gas channels are also solved as user-

defined scalars. The electrochemical reactions occurring in the catalyst layers are modeled through

various source terms while other model parameters are handled through the user interface. The PEMFC

model can be used in parallel ANSYS Fluent as well.

Note the following limitation when using the PEMFC model:

The anisotropic species diffusivity option is not compatible with the PEMFC model.

Due to the fact that there are a number of different physical zones associated with the fuel cell, the

following regions must be present in the fuel cell mesh (see Figure . : Schematic of a PEM Fuel Cell):

Anode flow channel

Anode gas diffusion layer

Anode micro-porous layer (optional)

Anode catalyst layer

Membrane layer (solid)

Cathode catalyst layer

Cathode micro-porous layer (optional)

Cathode gas diffusion layer

Cathode flow channel

The following zones have to be identified, if present in the fuel cell mesh:

Anode current collector (solid)

Cathode current collector (solid)

Coolant channel

The PEMFC model is provided as an add-on module with the standard ANSYS Fluent licensed software.

The module is installed with the standard installation of ANSYS Fluent in a directory called addons/pem-

fc in your installation area. The PEMFC module consists of a UDF library and a pre-compiled Scheme

library, which must be loaded and activated before calculations can be performed.

The PEMFC module is loaded into ANSYS Fluent through the text user interface (TUI). The module can

only be loaded after a valid ANSYS Fluent case file has been set or read. The text command to load

the add-on module is

Modeling Fuel Cells

Fluent  Addon Modules:

. None

. MHD Model

. Battery Module

. MSMD Battery Model

Select the PEM Fuel Cell Model by entering the module number . During the loading process, a

Scheme library (containing the graphical and text user interface) and a UDF library (containing a set

of user defined functions) are loaded into ANSYS Fluent.

The PEMFC model can be used to model polymer electrolyte membrane fuel cells (PEMFC). The following

describes an overview of the procedure required in order to use the PEMFC model in ANSYS Fluent.

You must start ANSYS Fluent in 3D double-precision mode. Note that the PEMFC model is only

available in 3D.

. Read the case or mesh file.

. Scale the mesh, if necessary.

. Use the PEM Fuel Cell Model dialog box to define the fuel cell model parameters.

Important

The PEM Fuel Cell Model dialog box greatly simplifies the input of parameters and

boundary conditions, but it does not replace the boundary conditions interface. Therefore,

Using the PEMFC Model

it is a good policy to start the setup with the PEM Fuel Cell Model dialog box and do the

finishing steps for boundary conditions afterwards.

Important

Note that the majority of this chapter describes how to set up the ANSYS Fluent PEMFC

model using the graphical user interface. You can also perform various tasks using the text

user interface. For more information, see Using the PEMFC Text User Interface.

Once the module has been loaded, in order to set fuel cell model parameters and assign properties

to the relevant regions in your fuel cell, you need to access the fuel cell graphical user interface (the

PEM Fuel Cell Model dialog box).

To open the PEM Fuel Cell Model dialog box: In the Outline View, under the Models branch, right-

click PEM Fuel Cel and select Edit... in the menu that opens.

Setup → Models → PEM Fuel Cell

Edit...

Figure . : The PEMFC Option in the Outline View

By default, the PEMFC model is enabled.

Using the PEM Fuel Cell Model dialog box, you can identify the relevant zones for the current collectors,

flow channels, gas diffusion layers, micro porous layers, catalyst layers, and the electrolyte (membrane).

You can specify the following inputs using the PEM Fuel Cell Model dialog box. Optional inputs are

indicated as such.

. Set the appropriate options for the fuel cell model.

. Set the various parameters for the fuel cell model.

. Select the appropriate zones and specify the properties on the anode side.

. Select the appropriate zones and specify the properties of the electrolyte/membrane.

. Select the appropriate zones and specify the properties on the cathode side.

. Provide input for advanced features such as contact resistivities, coolant channel properties, or stack

management settings (optional).

. Set solution controls such as under-relaxation factors (optional).

. Provide input to assist reporting (optional).

Refer to the following sections for more information:

.... Specifying Model Options (Model Tab)

.... Specifying Model Parameters (Parameters Tab)

.... Specifying Anode Properties (Anode Tab)

.... Specifying Electrolyte/Membrane Properties (Electrolyte Tab)

.... Specifying Cathode Properties (Cathode Tab)

.... Setting Advanced Properties (Advanced Tab)

.... Reporting on the Solution (Reports Tab)

The Model tab of the PEM Fuel Cell Model dialog box allows you to select or cancel the selection

of various options when solving a fuel cell problem.

Figure . : The Model Options in the PEM Fuel Cell Model Dialog Box

Options

Several fuel cell model options are available including:

Joule Heating

takes into account ohmic heating.This option includes the

terms in the energy source term in the

Options

calculations. See Table . :Volumetric Heat Source Terms for the list of additional volumetric sources

in the thermal energy equation.

Reaction Heating

takes into account the heat generated by the electrochemical reactions.

Electrochemistry Sources

allows the PEMFC model to take electrochemistry effects into account. If you are only interested in the

basic flow field throughout the fuel cell, you can turn off the Electrochemistry Sources option in order

to suppress most effects of the PEMFC model.You may also turn off the effect of these sources in order

to obtain a fluid flow initially, and then turn it back on.

Butler-Volmer Rate

(the default) is used to compute the transfer currents inside the catalyst layers. If this option is turned

off, the Tafel approximation (Equation . and Equation .) is used.

Liquid Phase

takes into account liquid phase calculations. Use this option if you are solving for liquid transport in the

fuel cell.

Multicomponent Diffusion

is used to compute the gas species mass diffusivity using the full multicomponent diffusion method as

described in Equation ., as opposed to the default option that uses Equation ..

Anisotropic E-Cond. in Porous Electrode

is used to model the typically non-isotropic electrical conductivity. It is applicable only for porous elec-

trodes (gas diffusion layers and micro porous layers).

Due to the fibrous structure of the porous material that is used for the electrodes (or gas diffusion

layer), the electrical conductivity is typically non-isotropical, with the cross-plane components

being orders of magnitude smaller than the in-plane components. This can be modeled using

the Anisotropic E-Conductivity in Porous Electrode setting. When this option is enabled, the

Electrical Conductivity for the solid material used in the porous electrodes is no longer used.

Instead, you need to specify, for this solid material, the electrical conductivity by choosing one

of the three non-isotropical options for the UDS diffusivity (UDS-). The three options are: aniso-

tropic; orthotropic; and cyl-orthotropic. For more information about these UDS Diffusivity options,

refer to the ANSYS Fluent User's Guide (p. ).

For example, to use this feature, perform the following steps:

Select the Anisotropic E-Conductivity in Porous Electrode option in the Model tab of the PEM Fuel

Cell Model dialog box.

In the Create/Edit Materials dialog box, select defined-per-uds for UDS Diffusivity for the solid

material that is to be used for the porous electrode.

Select one of the three options for UDS-: anisotropic; orthotropic; or cyl-orthotropic and set the

appropriate values.

Important

Note that, in this case, the Electrical Conductivity for this solid material is ignored.

Effective P-Cond. in MEA

enables the computation of the electrolyte phase conductivity

with consideration of ionomer

volume fraction and tortuosity in the catalyst layers using Equation .. If this option is disabled, then

and

.

Use Half-Cell Potentials

enables the calculations of the anode and cathode half-cell potentials

and

using the Nernst

equations (Equation . and Equation . ). If this option is disabled, the constant open-circuit voltage

is assumed, and the

and

are set to zero.

and

and

Cathode Particle Model

enables the cathode particle model. For information about this model, see The Cathode Particle Model.

enables the liquid water transport equations in the computations. By default, this option is enabled.

Compute Liquid in Channels

enables the solution of the liquid saturation equation in the gas channels. By default, this option is dis-

abled, and the equation is not solved.

Include Dynamic Head

(if enabled) includes the dynamic pressure in the gas channel in Equation ..

W-Diff Model

You can select one of the following formulations for the function

in Equation . :

Wu

computes

using Wu's formulation (Equation . ).

Wang

computes

using Wang's formulation (Equation . ).

Under-Relaxation Factors

You can use the Under-Relaxation Factors fields to influence the solution process.

Liquid-Vapor

The source term

in Equation . usually requires under-relaxation. Since the

is computed expli-

citly as a source term for the capillary pressure equation (Equation . ), the under-relaxation factor

usually must be a small value in order to obtain convergence.You can change the default value for the

under-relaxation factor by changing the value for Liquid-Vapor.

Disv’d-Vapor/Liquid

The source terms

and

in Equation . usually require under-relaxation also.You can change

the default value for the under-relaxation factor by changing the value for Disv’d-Vapor/Liquid.

Osmotic Drag Source

You can also specify an under-relaxation factor for the osmotic drag term, namely the left-hand side

term of Equation . by changing the value for Osmotic Drag Source.

GDL Liquid Removal

The liquid water flux that goes out of the gas diffusion layer (GDL) at the GDL-Channel interface (Equa-

tion .) can also be under-relaxed using GDL Liquid Removal.

Automatic Settings

The following parallel multigrid solver control parameter is available:

F-cycle for All Equations

sets the multigrid cycle type to F cycle for all equations that are being solved.This control overrides the

equation cycle settings in the Advanced Solution Controls dialog box.

Note

Using F-cycle for PEMFC computations is the best practice approach.

You can use the Parameters tab of the PEM Fuel Cell Model dialog box to specify the electrochemistry

parameters for the PEMFC model, reference diffusivities for the reactants and other model parameters.

Figure . : The Parameters Tab of the PEM Fuel Cell Model Dialog Box

Electrochemistry

There are various parameters under Electrochemistry in the PEM Fuel Cell Model dialog box. For

both the anode and the cathode, you can set the following parameters or leave the default values:

J_ref

and

, the reference exchange current density from Equation . and Equa-

tion ..

C_ref

corresponds to the reference concentration (

and

) with units of  kgmol/m3 (see Equa-

tion . and Equation . ).

Con. Exponent

corresponds to , the concentration dependence from Equation ..

Exch. Coeff. (a) , Exch. Coeff. (c)

are the transfer coefficients

and

from Equation . and Equation ., respectively.

Std. State E0

and

are the reversible potentials

and

in Equation . and Equation ., respectively.This field

appears only when Use Half-Cell Potentials option is selected under the Model tab.

Entropy

is the reaction entropy

and

in Equation . and Equation ..

V_Open

corresponds to the constant value assigned to cathode half-cell potential

and

.This parameter

appears only when Use Half-Cell Potentials option is not selected under the Model tab.

I_leak

is the leakage current density (A/m2). It is used to compute the total leakage current  (in Equation .

through Equation .) by:

where

is the electrolyte projected area (specified under the Reports tab). When leakage through

the electrolyte occurs, the fuel cell generates less current especially for cases with low values of

fuel or air utilization. Note that you can also specify the total leakage current through the user-

defined function Leakge_Current(). For more information, see User-Accessible Func-

Std.Temp. for U0 (K)

is the reference standard state temperature which is used for half-cell potentials computations in the

Nernst equations (Equation . and Equation . ).This parameter appears only when the Use Half-

Cell Potentials option is selected under the Model tab.

Std. Press. for U0 (Pa)

is the reference standard state pressure which is used for half-cell potentials computations in the Nernst

equations (Equation . and Equation . ).This parameter appears only when the Use Half-Cell

Potentials option is selected under the Model tab.

Note

The default values of the model parameters are determined based on various data available

Note

in the literature (, ,  , and others).

Reference Diffusivity

The parameters in the Reference Diffusivity group box appear only if the Multicomponent Diffusion

option is turned off in the Model tab. These parameters correspond to the species mass diffusivity

from Equation ..

When the Liquid Phase option is selected under the Model tab, you can specify the following para-

meters that appear in the Liquid Phase group box:

Expon’t Diff_gas

from Equation . for multiphase PEMFC calculations.

Expon’t J_ref

is the exponent

that is used to modify

and

according to Equation . to account for liquid

blockage to the reaction surface in Equation . through Equation ..

Expon’t K_rel

is the exponent  that is used to compute the relative permeability in

(Equation . ).

Expon’t Liq_coverage

is the exponent  that is used to compute the phase-change rates

and

(Equation . and

Equation . ).

Liq.-Disv’ed Phase

is the mass exchange rate constant

that is used to compute the rate of mass change between liquid

and dissolved phases

Liquid Density , Liq.Thermal Cond.

are the density

and thermal conductivity

of liquid water, respectively. Note that the effective thermal

conductivity in porous media is computed as:

(.)

Liq. Diff. in Chan.

is the

in Equation ..This parameter appears only when the Compute Liquid In Channel option

is selected under the Model tab.

V_liq/V_gas in Chan.

is the liquid to gas velocity ratio in the channel (  in Equation . ).This parameter appears only when

the Compute Liquid In Channel option is selected under the Model tab.

Other Parameters

Under Other Parameters, you can specify the following:

Gas-Disv’ed Phase

that is used to compute the rate of mass change between gas

Mod. Coef. OSM_drag

is the constant

with the default value of . that is used to generalize the default osmotic drag

Eq.W. Cont. at a=

is the equilibrium water content at the water activity of ,

, that is used in computing the equilibrium

water content

Eq.W. Cont. at s=

is the equilibrium water content at water saturation of ,

(Equation . ).This item appears only if the Liquid Phase option is selected under

the Model tab.

You can use the Anode tab of the PEM Fuel Cell Model dialog box to specify zones and properties

of the current collector, the flow channel, the diffusion layer, the micro porous layer (optional), and

the catalyst layer for the anode portion of the fuel cell.

..... Specifying Current Collector Properties for the Anode

Figure . : The Anode Tab of the PEM Fuel Cell Model Dialog Box with Current Collector

Selected

. Under Anode Zone Type, select Current Collector.

. From the Zone(s) selection list, select a corresponding zone. If you are modeling a fuel cell stack, then

you must select all zones of a particular type as a group.

. From the Solid Material drop-down list, select the appropriate material.You can use the Create/Edit

Materials dialog box to customize solid materials. Note that for the Electrical Conductivity, you can

only select a constant value in the Create/Edit Materials dialog box.The solid electrical conductivity

value is the diffusivity of the solid phase potential in the solid zones.

..... Specifying Flow Channel Properties for the Anode

Figure . : The Anode Tab of the PEM Fuel Cell Model Dialog Box with Flow Channel Selected

. Under Anode Zone Type, select Flow Channel.

. From the Zone(s) selection list, select an appropriate zone.

..... Specifying Porous Electrode Properties for the Anode

Figure . : The Anode Tab of the PEM Fuel Cell Model Dialog Box with Porous Electrode

Selected

. Under Anode Zone Type, select Porous Electrode.

. Specify values for the following parameters:

Porosity

is  in Equation ..

Absolute Permeability

is

H-phobic Contact Angle

hydrophobic contact angle

Water Removal Coef.

Leverett Func. Coeff_a

is

is the Leverett function coefficient  in Equation . (default = . ).

Leverett Func. Coeff_b

Leverett Func. Coeff_c

Condensation Rate Coeff.

Evaporation Rate Coeff.

..... Specifying Catalyst Layer Properties for the Anode

Figure . : The Anode Tab of the PEM Fuel Cell Model Dialog Box with TPB Layer (Catalyst)

Selected

. Under Anode Zone Type, select TPB Layer (Catalyst).

Porosity

is

Surface/Volume Ratio

is the specific active surface area  in Equation ..

is the hydrophobic contact angle

Protonic Conduction Coefficient

is the model constant

in Equation . (available only when the Effective P-Conductivity in

MEA option is selected under the Model tab).

Protonic Conduction Exponent

Ionomer Tortuosity

is the

in Equation . (available only when the Effective P-Conductivity in MEA option is se-

lected under the Model tab).

Ionomer Volume Fraction

is the

Activation Energy for P-Cond

is the

Activation Energy for J_ref

is the

Reference Temperature Temperature for J_ref

is the

..... Specifying Micro Porous Layer (Optional) Properties for the Anode

Figure . : The Anode Tab of the PEM Fuel Cell Model Dialog Box with Micro Porous Layer

Selected

. Under Anode Zone Type, select Micro Porous Layer.

Porosity

is

..... Specifying Cell Zone Conditions for the Anode

For each case of the anode’s current collector, diffusion layer, micro porous layer, and catalyst layer,

you assign a solid material and/or set the porosity and the viscous resistance. These settings represent

setting a cell zone condition. With the Update Cell Zones option turned on (the default setting),

this cell zone condition is applied to all selected zones in the Zone(s) list. If you want to set the cell

zone conditions for each zone individually (using the Cell Zone Conditions task page), you should

turn off the Update Cell Zones option.

You can use the Electrolyte tab of the PEM Fuel Cell Model dialog box to specify zones and properties

of the electrolyte/membrane portion of the fuel cell.

Figure . : The Electrolyte Tab of the PEM Fuel Cell Model Dialog Box

Materials dialog box to customize solid materials.

Equivalent Weight

is the

is the

is the

Water Diffusivity Coefficient

is the

is the

is the

Note that the PEMFC model allows you to model the electrolyte/membrane as a solid zone only.

However, it still allows for dissolved water, liquid or capillary pressure, and the ionic current to pass

through.

..... Specifying Cell Zone Conditions for the Membrane

When you assign a solid material to the membrane, you are setting a cell zone condition. With the

Update Cell Zones option turned on (the default setting), this cell zone condition is applied to all

selected zones in the Zone(s) list. If you want to set the cell zone conditions for each zone individually

(using the Cell Zone Conditions task page), you should turn off the Update Cell Zones option.

You can use the Cathode tab of the PEM Fuel Cell Model dialog box to specify zones and properties

of the current collector, the flow channel, the diffusion layer, the micro porous layer, and the catalyst

layer for the cathode portion of the fuel cell.

..... Specifying Current Collector Properties for the Cathode

The procedure for specifying the current collector properties for the cathode is similar to that for

the anode. For specific steps, refer to Specifying Current Collector Properties for the Anode (p. )

for details and then substitute “cathode” for “anode” where appropriate.

..... Specifying Flow Channel Properties for the Cathode

The procedure for specifying the flow channel properties for the cathode is similar to that for the

anode. For specific steps, refer to Specifying Flow Channel Properties for the Anode (p. ) and then

substitute “cathode” for “anode” where appropriate.

..... Specifying Porous Electrode Properties for the Cathode

The procedure for specifying the porous electrode properties for the cathode is similar to that for

the anode. For specific steps, refer to Specifying Porous Electrode Properties for the Anode (p. )

and then substitute “cathode” for “anode” where appropriate.

..... Specifying Catalyst Layer Properties for the Cathode

Figure . : The Cathode Tab of the PEM Fuel Cell Model Dialog Box with TPB Layer (Catalyst)

Selected

. Under Cathode Zone Type, select TPB Layer (Catalyst).

Selected

Porosity

is

is the

is the

is the

is the

is the

Reference Temperature for J_ref

is the

Besides the parameters for the catalyst layer listed above, you can also specify the following

parameters for The Cathode Particle Model:

Prod. Of O2 Solubility and Diffusivity

is

Radius of Catalyst Particle

is

Cathode Ionomer Resistance

is

..... Specifying Micro Porous Layer (Optional) Properties for the Cathode

The procedure for specifying the catalyst layer properties for the cathode is similar to that for the

anode. For specific steps, refer to Specifying Micro Porous Layer (Optional) Properties for the An-

ode (p. ) and then substitute “cathode” for “anode” where appropriate.

..... Specifying Cell Zone Conditions for the Cathode

For each case of the cathode’s current collector, diffusion layer, micro porous layer, and catalyst

layer, you assign a solid material and/or set the porosity and the viscous resistance. These settings

represent setting a cell zone condition. With the Update Cell Zones option turned on (the default

setting), this cell zone condition is applied to all selected zones in the Zone(s) list. If you want to

set the cell zone conditions for each zone individually (using the Cell Zone Conditions task page),

you should turn off the Update Cell Zones option.

You can use the Advanced tab of the PEM Fuel Cell Model dialog box to specify the contact resistivity

for any material interface in the geometry, set parameters for coolant channels, and define fuel stack

units for managing stacks of fuel cells.

..... Setting Contact Resistivities for the PEMFC Model

Figure . : The Advanced Tab of the PEM Fuel Cell Model Dialog Box for Contact Resistivities

. Under Advanced Setup, select Contact Resistivity.

. From the Available Zone(s) selection list, select any number of corresponding interfaces.These zones

are face zones over which a jump in electrical potential is caused by imperfect conduction.

Note

The contact resistance will be applied only to wall and porous jump types of in-

terfaces.

. Specify a value for the Resistivity for each specified zone.

Note that at porous jump and wall/wall-shadow interfaces, the contact resistivity is applied at

each face. Therefore, you need to specify the resistivity only at one of the interface walls, otherwise

the actual resistance will be doubled at the interface.

. To simplify the input, you can choose to use the resistivity value of the first selected zone for all others

as well by selecting the Use First Value for All option.

..... Setting Coolant Channel Properties for the PEMFC Model (Optional)

Figure . : The Advanced Tab of the PEM Fuel Cell Model Dialog Box for the Coolant Channel

. Under Advanced Setup, select Coolant Channel.

. From the Zone(s) selection list, select any number of corresponding zones.

. Specify a value for the Coolant Density.

. To enable the coolant channel, select the Enable Coolant Channel(s) option. Amongst other settings,

this will automatically create a new mixture material pem+cool-mixture consisting of hydrogen,

oxygen, water-vapor, coolant-liquid, and nitrogen.

. Using the Create/Edit Materials dialog box, set all other material properties for the new fluid coolant-

liquid.

. Specify the inlet and outlet conditions for cooling channels using standard boundary conditions dialog

boxes.

..... Managing Stacks for the PEMFC Model

Figure . : The Advanced Tab of the PEM Fuel Cell Model Dialog Box for Stack Management

The ANSYS Fluent PEMFC model allows you to model fuel cell stacks as well as individual fuel cells.

In the Advanced tab of the PEM Fuel Cell Model dialog box, you can define fuel cell units for each

fuel cell in a stack. A fuel cell unit consists of all zones of a single fuel cell in the stack.

Important

If you are only modeling a single fuel cell, then you do not need to set anything for Stack

Management in the Advanced tab of the PEM Fuel Cell Model dialog box.

. Select the Advanced tab of the PEM Fuel Cell Model dialog box.

. Select Stack Management under Advanced Setup.

. Since a fuel cell unit consists of all zones of a single fuel cell in the stack, select the corresponding zones

from the Zone(s) list.

. Create a new fuel cell unit by clicking the Create button.The new fuel cell is listed under Fuel Cell

Unit(s) with a default name.

. Edit a pre-existing fuel cell unit by selecting it in the Fuel Cell Unit(s) list.The zones in this fuel cell unit

are automatically selected in the Zone(s) list.You can then modify the zones that make up the fuel cell

unit and/or change its name in the Name field and click Modify to save the new settings.

. Remove a pre-existing fuel cell unit by selecting it in the Fuel Cell Unit(s) list and clicking the Delete

button.

Note

When deleting a unit, make sure that the electrical connectivity remains intact.

. If your model contains many zone names, you can use the Match Zone Name Pattern field to specify

a pattern to look for in the names of zones.Type the pattern in the text field and click Match to select

(or deselect) the zones in the Zones list with names that match the specified pattern.You can match

additional characters using * and ?. For example, if you specify wall*, all surfaces whose names begin

with wall (for example, wall-, wall-top) will be selected automatically. If they are all selected already,

they will be deselected. If you specify wall?, all surfaces whose names consist of wall followed by a

single character will be selected (or deselected, if they are all selected already).

For example, in a stack there are many fuel cells, say –, each having at least  zones (current

collector, gas channel, diffusion layer, and catalyst layer for both anode and cathode and a

membrane). Additionally, there may be coolant channels, and it may be that for mesh construction

reasons each of these physical zones is made up of more than one mesh zone. Even for small

stacks, you can easily end up having hundreds of cell zones in an ANSYS Fluent mesh. Therefore,

you may want to consider numbering the fuel cells in a stack and to use the assigned fuel cell

number in the names of the mesh zones. When you set up your stacked fuel cell case, you would

use the Match Zone Name Pattern field to pick all the zones belonging to a single fuel cell in

the stack, rather than scrolling through the potentially very long list and selecting them manually.

You can use the Reports tab of the PEM Fuel Cell Model dialog box to set up parameters that will

be useful in reporting data relevant to the fuel cell.

Figure . : The Reports Tab of the PEM Fuel Cell Model Dialog Box

The Electrolyte Projected Area field requires the projected area of the Membrane Electrolyte Assembly

(MEA) and is only used to calculate the average current density. The assembly consists of the membrane

and the catalyst layers above and below the membrane.

The External Contact Interface(s) fields require the face zones that act as external electrical contact

surfaces for the anode and the cathode.

These inputs are used to report cell voltage. For potentiostatic boundary conditions, this is the differ-

ence between the provided values, but for galvanostatic boundary conditions, the cell voltage is part

of the solution.

The following boundary conditions need to be defined for the PEMFC simulation based on your

problem specification:

Anode Inlet

– Mass flow rate

– Temperature

– Direction specification method

– Mass fractions (for example, h2, and h2o)

– The coolant must be set to zero if coolant channels are enabled

– UDS- (Water Saturation in Channels) must be set to zero

Cathode Inlet

– Mass fractions (for example o2, h2o, and n2)

Coolant Inlet (if any)

– Coolant mass fraction set to

Pressure Outlets (all)

Realistic backflow conditions.

Terminal Anode

– Temperature (or heat flux if known)

– UDS- (electric potential) set to ground voltage

Terminal Cathode

– UDS- (electric potential) is set to the voltage of the cathode (if solving to constant voltage), or the UDS-

(electric potential) flux is set to the current density in

(SI units) (if solving for constant current).

Note that the sign of the UDS- flux on the cathode side is negative.

For potentiostatic boundary conditions, after initialization, solutions are calculated easily for cell voltages

close to the open-circuit voltage. The same can be said for galvanostatic boundary conditions and low

electric current. By lowering the cell voltage or by raising the average electric current, you can calculate

subsequent stationary solutions.

In the event of convergence problems, it is recommended that you change the multigrid cycle to F-

cycle with BCGSTAB (bi-conjugate gradient stabilized method) selected as the stabilization method

for the species and the two potential equations. For the species and the user-defined scalar equations,

it may be necessary to reduce the termination (criteria) of the multigrid-cycles to

. For stack

simulations, the termination criterion may be reduced to

for the two potential equations.

Also, it may be useful to turn off Joule Heating and Reaction Heating in the PEM Fuel Cell Model

dialog box (in the Model tab) for the first few (approximately -) iterations after initialization. This

allows the two electric potentials to adjust from their initial values to more physical values, avoiding

the possibility of extreme electrochemical reactions and electric currents that would in turn adversely

impact the solution.

scalars and user-defined memory allocations. By default, the ANSYS Fluent PEMFC model defines sev-

eral user-defined scalars and user-defined memory allocations, described in Table . : User-Defined

Scalar Allocations (p. ) and Table . : User-Defined Memory Allocations (p. ).

Electric Potential (solid phase potential) (Volts)

UDS

Protonic Potential (membrane phase potential) (Volts)

UDS

Capillary Pressure

UDS

Water Content

UDS

Liquid Saturation in Channels

UDS

X Current Flux Density (A/m2)

UDM

Y Current Flux Density (A/m2)

UDM

Z Current Flux Density (A/m2)

UDM

Current Flux Density Magnitude (A/m2)

UDM

UDS

UDM

UDM

UDM

UDM

Ohmic Heat Source (W/m3)

UDM

Reaction Heat Source (W/m3)

UDM

Overpotential (Volts)

UDM

Evaporation to Vapor Phase Change Source (kg/m3-s)

UDM

Osmotic Drag Coefficient

UDM

Water Activity

UDM

Equilibrium Water Content

UDM

Absorption from Vapor phase change source (kg/m3-s)

UDM

Absorption from Liquid Phase Change Source (kg/m3-s)

UDM

Transfer Current (A/m3)

UDM

Liquid Saturation in Porous Media

UDM

GDL Liquid Removal (kg/m3-s)

UDM

Osmotic Drag Source (kg/m3-s)

UDM

Capillary Pressure (Pa)

UDM

Pressure Gradient Source (kg/m3-s)

UDM

You can obtain this list by opening the Execute On Demand dialog box and pulling down the Function

User Defined → User Defined → Execute on Demand...

and access the execute-on-demand function called list_pemfc_udf.

Alternatively, you can view the listing that appears when you first load your PEMFC case, or you can

type list_pemfc_udf in the text user interface and the listing will appear in the console window.

Note

For field variables that are stored in UDM, use the corresponding variables for postpro-

cessing. Postprocessing the UDM itself is not recommended.

For reviewing simulation results in CFD-Post for cases involving UDM or UDS, export the

CFD-Post.

Important

When you load older PEM Fuel Cell cases into ANSYS Fluent, and you are monitoring a UDS

using volume or surface monitors, make sure you re-visit the corresponding monitors dialog

Important

box (for example, the Volume Monitor or the Surface Monitor dialog box) to verify that

the correct UDS name is used for the appropriate monitor.

As noted in Properties, you can directly incorporate your own formulations and data for the properties

of the fuel cell membrane using the pemfc_user.c source code file.

The following listing represents a description of the contents of the pemfc_user.c source code file:

real Get_P_sat(real T, cell_t c, Thread *t)

Returns the value of the water vapor saturation pressure as a function of temperature (Equation .)

or other user-specified values.

real Water_Activity(real P, real T, cell_t c, Thread *t)

Returns the value of water activity (Equation . ).

real Osmotic_Drag_Coefficient(cell_t c, Thread *t)

Returns the value of the osmotic drag coefficient (Equation . ).

real Membrane_Conductivity(real lam, cell_t c, Thread *t)

Returns the value of the protonic conductivity in MEA (Equation . ).

real Water_Content_Diffusivity(real lam, real T, real mem_mol_dens-

ity,cell_tc,Thread*t)

Returns the value of the water content diffusivity in the MEA (Equation . ).

real Gas_Diffusivity(cell_t c, Thread *t, int j_spe)

Returns the value of the gaseous species diffusivities in the channels, gas diffusion layers, micro porous

layers, and catalysts (Equation . ).

real MCD_Gas_Diffusivity(cell_t c, Thread *t, int i)

Returns the tortuosity-corrected value of the gas species diffusion coefficients computed with the mul-

ticomponent diffusion option (Equation . ).

real Compute_Js(real s, Thread *t)

Computes the Leverett function; namely, the

relation (Equation . ).

Real Capillary_P_Diffusivity(real sat, real K_abs, cell_t c, Thread *t)

Returns the

real Water_Content(cell_t c, Thread *t)

Computes the water content .

real Anode_AV_Ratio(cell_t c, Thread *t)

Returns the value of the specific active surface area (

in Equation .) for the anode catalyst.

real Cathode_AV_Ratio(cell_t c, Thread *t)

in Equation .) for the cathode catalyst.

real Anode_J_TransCoef(cell_t c, Thread *t)

Returns the value of the anode reaction reference current density

used in Equation ..

real Cathode_J_TransCoef(cell_t c, Thread *t)

Returns the value of the cathode reaction reference current density

real Open_Cell_Voltage(cell_t c, Thread *t)

Returns the value of the half-cell potential

used in Equation . and Equation ..

real Leakage_Current(cell_t c, Thread *t)

Returns the value of the total leakage current (  in Equation . through Equation . ).

real resistance_in_channel (real sat)

Returns momentum resistance as a function of liquid saturation in gas channels.

void Set_UDS_Names(char uds[n_uds_required][STRING_SIZE])

Used to rename user-defined scalars (UDSs). Note that the units of the user defined scalars cannot be

changed.

{

strncpy(uds[], "Electric Potential", STRING_SIZE-);

strncpy(uds[], "Protonic Potential", STRING_SIZE-);

strncpy(uds[], "Cap. Pressure", STRING_SIZE-);

{

strncpy(uds[], "Water Content", STRING_SIZE-);

strncpy(uds[], "Liq. Saturation in Channels",  STRING_SIZE-);

}

If you want to change the names of UDSs, change the second argument of the strncpy functions,

recompile and link the module as with any modification to pemfc_user.c. Note that

STRING_SIZE is fixed in pemfc.h and should not be changed.

Important

When you load older PEM Fuel Cell cases into ANSYS Fluent, and you are monitoring a

UDS using volume or surface monitors, make sure you re-visit the corresponding mon-

itors dialog box (for example, the Volume Monitor or the Surface Monitor dialog box)

to make sure that the correct UDS name is used for the appropriate monitor.

void Set_UDM_Names(char udm[n_udm_required][STRING_SIZE])

Used to rename user defined memory (UDMs). Note that the units of user defined memory cannot be

changed.

{

strncpy(udm[], "X Current Flux Density",  STRING_SIZE-);

strncpy(udm[], "Y Current Flux Density",  STRING_SIZE-);

strncpy(udm[], "Z Current Flux Density",  STRING_SIZE-);

strncpy(udm[], "Current Flux Density Magnitude", STRING_SIZE-);

strncpy(udm[], "Ohmic Heat Source", STRING_SIZE-);

strncpy(udm[], "Reaction Heat Source",  STRING_SIZE-);

strncpy(udm[], "Overpotential", STRING_SIZE-);

strncpy(udm[], "Evaporation to Vapor", STRING_SIZE-);

strncpy(udm[], "Osmotic Drag Coefficient", STRING_SIZE-);

strncpy(udm[], "Water Activity", STRING_SIZE-);

strncpy(udm[], "Equilibrium Water Content",  STRING_SIZE-);

strncpy(udm[], "Absorption from Vapor", STRING_SIZE-);

strncpy(udm[], "Absorption from Liquid", STRING_SIZE-);

strncpy(udm[], "Transfer Current",  STRING_SIZE-);

strncpy(udm[], "Liquid Saturation",  STRING_SIZE-);

strncpy(udm[], "GDL Liquid Removal",  STRING_SIZE-);

strncpy(udm[], "Osmotic Drag Source (PEM)", STRING_SIZE-);

strncpy(udm[], "Cap. Pressure", STRING_SIZE-);

strncpy(udm[], "Pressure Gradient Source", STRING_SIZE-);

}

If you want to change the names of UDMs, change the second argument of the strncpy functions,

Important

UDM using volume or surface monitors, make sure you re-visit the corresponding

monitors dialog box (for example, the Volume Monitor or the Surface Monitor dialog

box) to make sure that the correct UDM name is used for the appropriate monitor.

real electric_contact_resistance(face_t f, Thread *t, int ns)

Returns the value for the electrical contact resistance.

real Transfer_Current(real i_ref, real gamma, int species_i, real alpha_a,

real alpha_c, real *dRade, real *dRcde, Thread *t, cell_t c, real cath-

ode_volume)

Computes the transfer current (

), corresponding to

Inputs for this function include:

effective transfer current coefficient, computed by Cath-

ode_J_TransCoef(c,t) or Anode_J_TransCoef(c,t)

i_ref

cathode or anode concentration exponent

gamma

species index used in fuel cells (for example i_o2, i_h2, i_h2o)

species_i

i_ref

gamma

species_i

product of anode exchange coefficient and

alpha_a

product of cathode exchange coefficient and

alpha_c

current thread

t

current cell

c

total volume of cathode catalyst layer

cathode_volume

Outputs for this function include:

anode or cathode volumetric transfer current (

or

in Equation .)

source

partial derivative of

with respect to activation loss

dRade

dRcde

Thermal_ctk_pemfc(face_t f, Thread *t)

Used to change the constant value of Thermal Contact Resistance set in the Porous Jump dialog box

to a locally variable value.

Phase_Change_const(cell_t c, Thread *t)

Used to change the constant value of

used to compute the gas-liquid phase change rate.

.... Compiling the Customized PEMFC Source Code

This section includes instructions on how to compile a customized PEM Fuel Cell user-defined module.

Important

You will first want to use a local copy of the pemfc directory in the addons directory before you

recompile the PEM Fuel Cell module.

. Make a local copy of the pemfc directory. Do not create a symbolic link.

a.

Create a directory for the custom pemfc libraries (for example, /home/custom-build).

Important

a.

Important

The custom version of the library must be named according to the convention

used by ANSYS Fluent: for example, pemfc.

b. Copy the pemfc library from the installation of ANSYS Fluent (Ansys Inc\v195\fluent\flu-

. Change directories to the pemfc/src directory.

. Make changes to the pemfc_user.c file.

PEM Fuel Cell module.

. Change directories to the pemfc/ directory.

where arch is lnx86 on LINUX, or ultra on the Sun operating system, and so on.

the PEM Fuel Cell module that is located in a folder called home/sample.

cp -RH [ansys_inc/v195/fluent]/fluent19../addons/pemfc

/home/sample/pemfc

. Using a text editor, make the appropriate changes to the pemfc_user.c file located in

/home/sample/pemfc/src/pemfc_user.c

cd /home/sample/pemfc

..... Compiling the Customized Source Code under Windows

. Make a local copy of the pemfc folder. Do not create a shortcut.

a.

. Make sure that the $FLUENT_INC environment variable is correctly set to the current ANSYS Fluent

installation directory (for example, ANSYS Inc\v195\fluent).

. Enter the pemfc\src folder.

. Modify the pemfc_user.c file as desired and save the changes.

. Change your working directory to pemfc (for example, /home/custom-build/pemfc) and build

the custom addon library:

PEM Fuel Cell module in one of following ways:

The procedure for setting up and solving fuel cell problems using the Fuel Cell and Electrolysis Model

is described in detail in this chapter. Refer to the following sections for more information:

... Geometry Definition for the Fuel Cell and Electrolysis Model

... Installing the Fuel Cell and Electrolysis Model

... Loading the Fuel Cell and Electrolysis Module

...Workflow for Using the Fuel Cell and Electrolysis Module

... Setting Up the Fuel Cell and Electrolysis Module

... Modeling Current Collectors

... Fuel Cell and Electrolysis Model Boundary Conditions

... Solution Guidelines for the Fuel Cell and Electrolysis Model

... Postprocessing the Fuel Cell and Electrolysis Model

The ANSYS Fluent Fuel Cell and Electrolysis Model are made up of several user-defined functions

(UDFs) and a graphical user interface. The potential fields are solved as user-defined scalars. The liquid

water saturation, , and the water content,

, are also solved as user-defined scalars. The electrochem-

ical reactions occurring on the catalyst are modeled through various source terms while other model

parameters are handled through the user interface. The Fuel Cell and Electrolysis Model can be used

in parallel ANSYS Fluent as well.

Note the following limitation when using the Fuel Cell and Electrolysis model:

The anisotropic species diffusivity option is not compatible with the Fuel Cell and Electrolysis model.

following regions must be present in the fuel cell mesh:

Membrane layer

Anode current collector

Cathode current collector

The Fuel Cell and Electrolysis Model is provided as an add-on module with the standard ANSYS Fluent

licensed software. The module is installed with the standard installation of ANSYS Fluent in a directory

called addons/fuelcells in your installation area. The Fuel Cell and Electrolysis Model consists of

a UDF library and a pre-compiled Scheme library, which must be loaded and activated before calculations

can be performed.

The Fuel Cell and Electrolysis module is loaded into ANSYS Fluent through the text user interface (TUI).

The module can only be loaded after a valid ANSYS Fluent case file has been set or read. The text

command to load the add-on module is

. None

. MHD Model

Select the Fuel Cell and Electrolysis Model by entering the module number . During the loading

process, a Scheme library (containing the graphical and text user interface) and a UDF library (containing

a set of user defined functions) are loaded into ANSYS Fluent.

The Fuel Cell and Electrolysis Model can be used to model polymer electrolyte membrane fuel cells

(PEMFC), solid oxide fuel cells (SOFC), and the process of high-temperature electrolysis. The following

Using the Fuel Cell and Electrolysis Model

describes an overview of the procedure required in order to use the Fuel Cell and Electrolysis Model

in ANSYS Fluent.

. Read the case file.

. Use the Fuel Cell and Electrolysis Models dialog box to define the fuel cell model parameters.

Important

The Fuel Cell and Electrolysis Models dialog box greatly simplifies the input of parameters

and boundary conditions, but it does not replace the boundary conditions interface.

Therefore, it is a good policy to start the setup with the Fuel Cell and Electrolysis Models

dialog box and do the finishing steps for boundary conditions afterwards.

Important

Note that the majority of this chapter describes how to set up the ANSYS Fluent Fuel Cell

and Electrolysis Model using the graphical user interface. You can also perform various tasks

using the text user interface. For more information, see Using the Fuel Cell and Electrolysis

Text User Interface.

Fuel Cell and Electrolysis Models dialog box).

To open the Fuel Cell and Electrolysis Models dialog box: In the tree under the Models branch, right-

click Fuel Cells and Electrolysis and select Edit... in the menu that opens.

Setup → Models → Fuel Cells and Electrolysis

Edit...

Figure . : The Fuel Cell and Electrolysis Option in the Tree

By default, the PEMFC model is already enabled, however, you can also choose the SOFC or the Elec-

trolysis models.

Using the Fuel Cell and Electrolysis Models dialog box, you can identify the relevant zones for the

current collectors, flow channels, gas diffusion layers, catalyst layers, and the membrane/electrolyte.

You can specify the following inputs using the Fuel Cell and Electrolysis Models dialog box. Optional

inputs are indicated as such.

. Enable the appropriate type of fuel cell model, either PEMFC, SOFC, or Electrolysis.

. Enable either the single-phase or the multi-phase fuel cell model (if PEMFC is selected).

. Set the appropriate options for the fuel cell model (optional).

. Select the appropriate zones and specify the properties of the membrane/electrolyte.

The Model tab of the Fuel Cell and Electrolysis Models dialog box allows you to turn on or off

various options when solving a fuel cell problem. To model polymer electrolyte membrane fuel cells,

enable the PEMFC option in the Model tab. Likewise, to model solid oxide fuel cells, enable the SOFC

option in the Model tab. Finally, to model electrolysis, enable the Electrolysis option in the Model

tab.

Figure . : The Model Options in the Fuel Cell and Electrolysis Models Dialog Box—PEMFC

Enabled

Several fuel cell model options are available in the Model tab of the Fuel Cell and Electrolysis

Models dialog box including:

The Joule Heating option takes into account ohmic heating.This option includes the

term in the energy

source term from Equation . in the calculations.

The Reaction Heating option takes into account the heat generated by the electrochemical reactions,

which includes the

term, and the product of transfer current and the over-potentials in the energy

The Electrochemistry Sources option allows the Fuel Cell and Electrolysis Model to take electrochemistry

effects into account. If you are only interested in the basic flow field throughout the fuel cell, you can turn

off the Electrochemistry Sources option in order to suppress most effects of the Fuel Cell and Electrolysis

Model.To turn off all effects of the Fuel Cell and Electrolysis Model, you should also turn off the Membrane

Water Transport and Multiphase options.

The Butler-Volmer Rate option (the default) is used to compute the transfer currents inside the catalyst

layers. If this option is turned off, the Tafel approximation (Equation .) is used.

The Membrane Water Transport option takes into account the transport of water across the membrane.

This option is only available for the PEMFC model.

The Multiphase option takes into account multiphase calculations. Use this option if you are solving for

approximate liquid transport in the gas diffusion layer of the fuel cell. (PEMFC only)

The Multicomponent Diffusion option is used to compute the gas species mass diffusivity using the full

multicomponent diffusion method as described in Equation ., as opposed to the default option that

The Anisotropic E-Conductivity in Porous Electrode option is used to model the typically non-isotropic

electrical conductivity. It is applicable only for porous electrodes (gas diffusion layers).

layer), the electrical conductivity is typically non-isotropical, with the cross-plane components being

orders of magnitude smaller than the in-plane components. This can be modeled using the Aniso-

tropic E-Conductivity in Porous Electrode setting. When this option is enabled, the Electrical

Conductivity for the solid material used in the electrolyte is no longer used. Instead, you need to

specify, for this solid material, the electrical conductivity by choosing one of the three non-isotrop-

ical options for the UDS diffusivity (UDS-). The three options are: anisotropic; orthotropic; and

cyl-orthotropic. For more information about these UDS Diffusivity options, refer to the ANSYS

Fluent User's Guide (p. ).

– Select the Anisotropic E-Conductivity in Porous Electrode option in the Model tab of the Fuel Cell

and Electrolysis Models dialog box.

– In the Create/Edit Materials dialog box, select defined-per-uds for UDS Diffusivity for the solid

– Select one of the three options for UDS-: anisotropic; orthotropic; or cyl-orthotropic and set the

Important

For PEMFC problems, you can use the Under-Relaxation Factors fields to influence the solution process.

The saturation source term

in Equation . usually requires under-relaxation. You can change

the default value for the under-relaxation factor by changing the value for Saturation Source.

The water content,

, in Equation . also may need under-relaxation. You can change the default

value for the under-relaxation factor by changing the value for Water Content.

Under Automatic Settings, the following parallel multigrid solver control parameters are available:

Enable Smooth Partition: Enables the smooth partitioning process when running in Parallel.

When this option is enabled, the fuel cell parallel solver:

– Uses the Metis method for partitioning the mesh

– Enables Laplace Smoothing

– Partitions and distributes the mesh data to all compute nodes

F-cycle for All Equations: Sets the multigrid cycle type to F cycle for all equations that are being solved.

This control overrides the equation cycle settings in the Advanced Solution Controls dialog box.

Nearly all options are turned on by default. You may want to override the default values, depending

on the problem you want to model. For instance, if you are not concerned with the heat generated

due to chemical reaction, then you may want to turn off the Reaction Heating option.

You can use the Parameters tab of the Fuel Cell and Electrolysis Models dialog box to specify the

electrochemistry parameters for the Fuel Cell and Electrolysis Model, reference diffusivities for the

reactants, among other model parameters.

Figure . : The Parameters Tab of the Fuel Cell and Electrolysis Models Dialog Box

There are various parameters under Electrochemistry in the Fuel Cell and Electrolysis Models dialog

box. For both the anode and the cathode, you can also set the following parameters or leave the

default values.

The Ref. Current Density corresponds to

and

, the reference exchange current density from

Equation . and Equation ..

The Ref. Concentration corresponds to the reference concentration (

and

) with units of

(see Equation . and Equation . ).

The Concentration Exponent corresponds to , the concentration dependence from Equation ..

The Exchange Coefficient (a) and Exchange Coefficient (c) correspond to the transfer coefficients,

and

, from Equation . and Equation ..

The Open-Circuit Voltage corresponds to

The Leakage Current corresponds to

in Equation . through Equation ..This is the total

amount of transfer current (A) due to fuel-oxidant cross-over (leakage through the electrolyte).When this

happens, the fuel cell generates less current especially for cases with low values of fuel or air utilization.

In addition to the constant value you can specify in the Electrochemistry tab, you can also specify the

leakage current through the user-defined function Leakge_Current(). For more information, see

User-Accessible Functions (p. ).

Moreover, the following parameters can also be set here:

The Reference Diffusivities correspond to

from Equation ., the species mass diffusivity.These

are not be required if the Multicomponent Diffusion option is enabled in the Model tab.

The Pore Blockage for Gas Diffusion corresponds to

from Equation . for multiphase PEMFC cal-

culations.

The Pore Blockage for Transfer Current is used to account for liquid blockage to the reaction surface

by modifying

and

in Equation . through Equation . as follows:

where  is the pore blockage for transfer current.

The Exponent for relative permeability corresponds to  in Equation ..

Note that, conventionally, the negative voltage is supplied to the cathode side in power consuming

devices such as electrolyzers. ANSYS Fluent adopts the inverse notation where the negative voltage

is supplied to the anode side whilst cathode remains positively charged. The main reason for this

discrepancy is that the same infrastructure is used for both the electrolysis and fuel cells models. Usage

of the terms "anode" and "cathode" in this manual and in the user interface should be interpreted

according to conventions for power-supplying devices.

You can use the Anode tab of the Fuel Cell and Electrolysis Models dialog box to specify zones

and properties of the current collector, the flow channel, the diffusion layer, and the catalyst layer

for the anode portion of the fuel cell.

Figure . : The Anode Tab of the Fuel Cell and Electrolysis Models Dialog Box With Current

Collector Selected

. Select the Anode tab of the Fuel Cell and Electrolysis Models dialog box.

. Select Current Collector under Anode Zone Type.

. Select a corresponding zone from the Zone(s) list. If you are modeling a fuel cell stack, then you must

pick all zones of a particular type as a group.

. Select a Solid Material from the corresponding drop-down list. Solid materials can be customized using

the Create/Edit Materials dialog box. Note that for the Electrical Conductivity, you can only choose

a constant value in the Create/Edit Materials dialog box.The solid electrical conductivity value is the

diffusivity of the solid phase potential in the solid zones.

Figure . : The Anode Tab of the Fuel Cell and Electrolysis Models Dialog Box With Flow

Channel Selected

. Select Flow Channel under Anode Zone Type.

. Select a corresponding zone from the Zone(s) list.

Figure . : The Anode Tab of the Fuel Cell and Electrolysis Models Dialog Box With Porous

Electrode Selected

. Select Porous Electrode under Anode Zone Type.

. Specify a value for the Porosity.

. Specify a value for the Viscous Resistance.

. Specify a value for the Contact Angle for multiphase fuel cell calculations (

Figure . : The Anode Tab of the Fuel Cell and Electrolysis Models Dialog Box With TPB

Layer (Catalyst) Selected

. Select TPB Layer (Catalyst) under Anode Zone Type.

. Specify a value for the Surface/Volume Ratio (the specific active surface area in Equation . ).

For each case of the anode’s current collector, diffusion layer, and catalyst layer, you assign a solid

material and/or set the porosity and the viscous resistance. These settings represent setting a cell

zone condition. With the Update Cell Zones option turned on (the default setting), this cell zone

condition is applied to all selected zones in the Zone(s) list. If you want to set the cell zone conditions

for each zone individually (using the Cell Zone Conditions task page), you should turn off the Update

Cell Zones option.

You can use the Electrolyte tab of the Fuel Cell and Electrolysis Models dialog box to specify zones

and properties of the electrolyte/membrane portion of the fuel cell.

Figure . : The Electrolyte Tab of the Fuel Cell and Electrolysis Models Dialog Box

pick all membrane zones as a group.

the Create/Edit Materials dialog box.

. Specify a value for the Equivalent Weight (

. Specify a value for the Protonic Conduction Coefficient (  in Equation . ).This is used to calculate

the membrane phase electric conductivity.

. Specify a value for the Protonic Conduction Exponent (

Note that the Fuel Cell and Electrolysis Model allows you to model the electrolyte/membrane as either

a fluid zone or as a solid zone. For PEMFC, the Fuel Cell and Electrolysis Model still allows for water

and the ionic current to pass through the electrolyte/membrane.

You can use the Cathode tab of the Fuel Cell and Electrolysis Models dialog box to specify zones

for the cathode portion of the fuel cell.

Figure . : The Cathode Tab of the Fuel Cell and Electrolysis Models Dialog Box With Current

. Select the Cathode tab of the Fuel Cell and Electrolysis Models dialog box.

. Select Current Collector under Cathode Zone Type.

Figure . : The Cathode Tab of the Fuel Cell and Electrolysis Models Dialog Box With Flow

. Select Flow Channel under Cathode Zone Type.

Figure . : The Cathode Tab of the Fuel Cell and Electrolysis Models Dialog Box With Porous

. Select Porous Electrode under Cathode Zone Type.

Figure . : The Cathode Tab of the Fuel Cell and Electrolysis Models Dialog Box With TPB

. Select TPB Layer(Catalyst) under Cathode Zone Type.

For each case of the cathode’s current collector, diffusion layer, and catalyst layer, you assign a solid

You can use the Advanced tab of the Fuel Cell and Electrolysis Models dialog box to specify the

contact resistivity for any material interface in the geometry, set parameters for coolant channels,

and define fuel stack units for managing stacks of fuel cells.

..... Setting Contact Resistivities for the Fuel Cell and Electrolysis Model

Figure . : The Advanced Tab of the Fuel Cell and Electrolysis Models Dialog Box for Contact

Resistivities

. Select the Advanced tab of the Fuel Cell and Electrolysis Models dialog box.

. Select Contact Resistivity under Advanced Setup.

. Select any number of corresponding interfaces from the Available Zone(s) list.These zones are face

zones over which a jump in electrical potential is caused by imperfect conduction.

as well by turning on the Use First Value for All option.

..... Setting Coolant Channel Properties for the Fuel Cell and Electrolysis Model

Figure . : The Advanced Tab of the Fuel Cell and Electrolysis Models Dialog Box for the

Coolant Channel

. Select Coolant Channel under Advanced Setup.

. Select any number of corresponding zones from the Zone(s) list.

. Specify a value for the Density.

. Specify a value for the Heat Capacity.

. Specify a value for the Thermal Conductivity.

. Specify a value for the Viscosity.

. To enable the coolant channel, turn on the Enable Coolant Channel(s) option. Amongst other settings,

this will change the mixture to include the coolant species, which is otherwise absent.

..... Managing Stacks for the Fuel Cell and Electrolysis Model

Figure . : The Advanced Tab of the Fuel Cell and Electrolysis Models Dialog Box for Stack

Management

The ANSYS Fluent Fuel Cell and Electrolysis Model allows you to model fuel cell stacks as well as

individual fuel cells. In the Advanced tab of the Fuel Cell and Electrolysis Models dialog box, you

can define fuel cell units for each fuel cell in a stack. A fuel cell unit consists of all zones of a single

fuel cell in the stack.

Important

Management in the Advanced tab of the Fuel Cell and Electrolysis Models dialog box.

button.

. You can have ANSYS Fluent attempt to automatically determine the zones that constitute a single fuel

cell in a stack using the Suggest Stack Setup button. Manually performing this task is often time-con-

suming and error-prone. Using the Suggest Stack Setup button can save you from having to manually

enter this information yourself for potentially hundreds of zones.

When using the Suggest Stack Setup button, ANSYS Fluent needs to correctly identify electrically

conducting parts and their connectivity (anode, electrolyte, cathode, coolant channels, and ex-

ternal contacts) using zone information generally required by the fuel cell model anyway. ANSYS

Fluent requires zone information to have been specified in all of the following tabs in the Fuel

Cell and Electrolysis Models dialog box:

In the Anode tab, specify zone information for the current collector, the porous electrode, and the

TPB catalyst layer.

In the Electrolyte tab, specify zone information for the electrolyte/membrane.

In the Cathode tab, specify zone information for the current collector, the porous electrode, and the

In the Advanced tab, specify zone information for the coolant channel.

In the Reports tab, specify the external contact interface(s).

In the Advanced tab, click the Suggest Stack Setup button.

Important

If your fuel cell model inputs are incorrect (or incomplete), ANSYS Fluent cannot

completely be sure that the resulting setup is correct. Also, even if your inputs are

correct, an unconventional fuel cell design may cause ANSYS Fluent to suggest an

inaccurate stack setup. So, it is your responsibility to verify the stack setup prior to

clicking either the OK or the Apply buttons.

You can use the Reports tab of the Fuel Cell and Electrolysis Models dialog box to set up parameters

that will be useful in reporting data relevant to the fuel cell.

Figure . : The Reports Tab of the Fuel Cell and Electrolysis Models Dialog Box

and the catalyst layers above and below the membrane. The value of the projected area can be

computed from the Projected Surface Areas dialog box.

Results → Reports → Projected Areas

Edit...

The External Contact Interface(s) fields requires the face zones that act as external contact surfaces

for the anode and the cathode.

In previous versions of ANSYS Fluent, user-defined scalar (UDS) equations could only be solved in fluid

zones. This restriction is now removed. As a result, the Fuel Cell and Electrolysis module allows you to

model current collectors as solid, as well as fluid zones. One advantage of using solids as the current

collector is that the convergence of the species equations are not hindered by the potentially skewed

mesh inside the current collectors.

If fluid zones are used to model solid current collectors, ANSYS Fluent automatically sets velocities to

zero and cuts off species transport into these zones. If solid zones are used, however, you need to ac-

tivate the solution of the electric potential (UDS-) in these solid zones (see the separate ANSYS Fluent

User’s Guide for details). The value of the Electrical Conductivity for the solid material must be assigned

in the Create/Edit Materials dialog box.

Figure . : The Electric Conductivity Field in the Create/Edit Materials Dialog Box

Important

Note that the UDS Diffusivity should be set to user-defined (cond::fuelcells).

Do not use the defined-per-uds option.

For more information on the user-defined scalar diffusivity, see the separate ANSYS Fluent User's

Note that the Fuel Cell and Electrolysis Model allows you to model current collectors either as porous

media zones (if you want to allow for mass and momentum transport within the collectors) or as solid

zones.

zones.

The following boundary conditions need to be defined for the Fuel Cell and Electrolysis simulation

based on your problem specification:

– Mass fractions (for example, h2, and h2o).

– The coolant must be set to zero if coolant channels are enabled.

– UDS- (Water Saturation) must be set to

– Mass fractions (for example o2, h2o, and n2).

– Temperature (or flux if known)

For potentiostatic boundary conditions, after initialization, steady-state solutions are calculated easily

for cell voltages close to the open-circuit voltage. The same can be said for galvanostatic boundary

conditions and low electric current. By lowering the cell voltage or by raising the average electric

current, you can calculate subsequent stationary solutions.

. For stack

Also, it may be useful to turn off Joule Heating and Reaction Heating in the Fuel Cell and Electro-

lysis Models dialog box (in the Model tab) for the first few (approximately -) iterations after initial-

ization. This allows the two electric potentials to adjust from their initial values to more physical values,

avoiding the possibility of extreme electrochemical reactions and electric currents that would in turn

adversely impact the solution.

scalars and user-defined memory allocations. By default, the ANSYS Fluent Fuel Cell and Electrolysis

Model defines several user-defined scalars and user-defined memory allocations, described in

Table . : User-Defined Scalar Allocations (p. ) and Table . : User-Defined Memory Alloca-

UDS

UDS

UDS

Water Saturation (liquid saturation)

UDS

UDS

X Current Flux Density (

)

UDM

Y Current Flux Density (

)

UDM

Z Current Flux Density (

)

UDM

Current Flux Density Magnitude (

)

UDM

Ohmic Heat Source (

)

UDM

Reaction Heat Source (

)

UDM

UDM

Phase Change Source (

)

UDM

UDM

Liquid Water Activity

UDM

Membrane Water Content

UDM

Protonic Conductivity (/ohm-m)

UDM

Back Diffusion Mass Source (

)

UDM

Transfer Current (

)

UDM

Osmotic Drag Source (

)

UDM

Alternatively, you can view the listing that appears when you first load your Fuel Cell and Electrolysis

case, or you can type list_pemfc_udf in the text user interface and the listing will appear in the

Note

CFD-Post.

Important

When you load older Fuel Cell and Electrolysis cases into ANSYS Fluent, and you are monit-

CFD-Post.

Important

oring a UDS using volume or surface monitors, make sure you re-visit the corresponding

monitors dialog box (for example, the Volume Monitor or the Surface Monitor dialog box)

to verify that the correct UDS name is used for the appropriate monitor.

of the fuel cell membrane using the pem_user.c source code file.

The following listing represents a description of the contents of the pem_user.c source code file:

real Water_Activity(realP, realT, cell_t c, Thread *t)

real Water_Content(real act)

Returns the value of the membrane water content at the membrane catalyst interface (Equation . ).

real Osmotic_Drag_Coefficient(real P, real T, cell_t c, Thread *t)

Returns the value of the membrane’s protonic conductivity (Equation . ).

real Electrolyte_Conductivity(cell_t c, Thread *t)

Returns the value of the ionic conductivity in the electrolyte (Equation . ). (SOFC and Electrolysis only)

Returns the value of the water content diffusivity in the membrane (Equation . ).

real Gas_Diffusivity(cell_tc, Thread *t, int j_spe)

Returns the value of the gaseous species diffusivities in the channels, gas diffusion layers and catalysts

real Saturation_Diffusivity(real sat, real cos_theta, real porosity, cell_t

c, Thread *t)

Returns the value of diffusivity of the liquid saturation. It computes the term

Returns the value of the open-circuit voltage

Returns the value of the leakage current (

in Equation . through Equation . ).

Used to rename user defined scalars (UDSs). Note that the units of the user defined scalars cannot be

changed.

{

changed.

{

strncpy(uds[], "Water Saturation",  STRING_SIZE-);

}

recompile and link the module as with any modification to pem_user.c. Note that STRING_SIZE

is fixed in pem.h and should not be changed.

Important

When you load older Fuel Cell and Electrolysis cases into ANSYS Fluent, and you are

monitoring a UDS using volume or surface monitors, make sure you re-visit the corres-

ponding monitors dialog box (for example, the Volume Monitor or the Surface Monitor

dialog box) to make sure that the correct UDS name is used for the appropriate monitor.

changed.

{

strncpy(udm[], "Phase Change Source (PEM)", STRING_SIZE-);

strncpy(udm[], "Osmotic Drag Coefficient (PEM)", STRING_SIZE-);

strncpy(udm[], "Liquid Water Activity (PEM)", STRING_SIZE-);

strncpy(udm[], "Membrane Water Content (PEM)",  STRING_SIZE-);

strncpy(udm[], "Protonic Conductivity", STRING_SIZE-);

strncpy(udm[], "Back Diffusion Source (PEM)", STRING_SIZE-);

}

Important

monitoring a UDM using volume or surface monitors, make sure you re-visit the corres-

dialog box) to make sure that the correct UDM name is used for the appropriate monitor.

real alpha_c, real *dRade, real *dRcde, Thread *t, cell_t c)

effective transfer current coefficient, computed by Cathode_J_TransCoef(c,t)

or Anode_J_TransCoef(c,t)

i_ref

gamma

species_i

alpha_a

alpha_c

t

c

species_i

alpha_a

alpha_c

t

c

in Equation . or

in

Equation .)

source

dRade

dRcde

Used to change the constant value of Thermal Contact Resistance for the porous zone set in the Porous

Jump dialog box to a locally variable value.

.... Compiling the Customized Fuel Cell and Electrolysis Source Code

This section includes instructions on how to compile a customized Fuel Cell and Electrolysis user-

defined module.

Important

You will first want to use a local copy of the fuelcells directory in the addons directory before

you recompile the Fuel Cell and Electrolysis module.

. Make a local copy of the fuelcells directory. Do not create a symbolic link.

Important

by ANSYS Fluent: for example, fuelcells.

. Change directories to the fuelcells/src directory.

. Make changes to the pem_user.c file.

Fuel Cell and Electrolysis module.

. Change directories to the fuelcells/ directory.

where your_arch is lnx86 on LINUX, or ultra on the Sun operating system, and so on.

the Fuel Cell and Electrolysis module that is located in a folder called home/sample:

cp -RH [ansys_inc/v195/fluent]/fluent19../addons/fuelcells

/home/sample/fuelcells

Using a text editor, make the appropriate changes to the pem_user.c file located in

/home/sample/fuelcells/src/pem_user.c

cd /home/sample/fuelcells

. Make a local copy of the fuelcells folder. Do not create a shortcut.

. Enter the fuelcells\src folder.

. Return to the fuelcells folder.

The procedure for setting up and solving solid oxide fuel cell (SOFC) problems (with unresolved electro-

lyte) is described in detail in this chapter. Refer to the following sections for more information:

... Limitation on Modeling Solid Oxide Fuel Cells

... Installing the Solid Oxide Fuel Cell With Unresolved Electrolyte Model

... Loading the Solid Oxide Fuel Cell With Unresolved Electrolyte Module

... Solid Oxide Fuel Cell With Unresolved Electrolyte Module Set Up Procedure

... Setting the Parameters for the SOFC With Unresolved Electrolyte Model

... Setting Up the Electrochemistry Parameters

... Setting Up the Electrode-Electrolyte Interfaces

... Setting Up the Electric Field Model Parameters

... User-Accessible Functions for the Solid Oxide Fuel Cell With Unresolved Electrolyte Model

The anisotropic species diffusivity option is not compatible with the Solid Oxide Fuel Cell model.

... Installing the Solid Oxide Fuel Cell With Unresolved Electrolyte

Model

The Solid Oxide Fuel Cell (SOFC) With Unresolved Electrolyte Model is provided as an addon module

with the standard ANSYS Fluent licensed software. The module is installed with the standard installation

of ANSYS Fluent in a directory called addons/sofc in your installation area. The SOFC With Unresolved

Electrolyte Model consists of a UDF library and a pre-compiled Scheme library, that must be loaded

and activated before calculations can be performed.

The Solid Oxide Fuel Cell (SOFC) With Unresolved Electrolyte Model is loaded into ANSYS Fluent through

the text user interface (TUI). The module can only be loaded after a valid ANSYS Fluent mesh or case

file has been set or read. The text command to load the addon module is

A list of ANSYS Fluent addon modules is displayed:

. None

. MHD Model

Using the Solid Oxide Fuel Cell With Unresolved Electrolyte Model

Select the SOFC With Unresolved Electrolyte Model by entering the module number . During the

loading process, a Scheme library (containing the graphical and text user interface) and a UDF library

(containing a set of user defined functions) are loaded into ANSYS Fluent.

Once the module has been loaded, the SOFC Model (Unresolved Electrolyte) option appears in the

tree under the Models branch and in the Models task page.

To enable the SOFC model: In the Outline View under the Models branch, right-click Fuel Cells and

Electrolysis and select Edit... in the menu that opens.

Setup → Models → SOFC Model (Unresolved Electrolyte)

Edit...

Figure . : Opening the SOFC Model Dialog Box in the Outline View

Edit...

When the SOFC Model dialog box appears, select the Enable SOFC Model option.

... Solid Oxide Fuel Cell With Unresolved Electrolyte Module Set Up

Procedure

The following describes an overview of the procedure required in order to use the SOFC With Unresolved

Electrolyte Model in ANSYS Fluent.

You must start ANSYS Fluent in 3D double-precision mode. Note that the SOFC With Unresolved

Electrolyte Model is only available in 3D.

. Scale the mesh.

Setup →

General → Scale...

. Define various model parameters for the simulation.

a.

Check the solver settings.

Setup →

General

i.

In the Solver group box, enable Pressure Based under Type.

ii.

Enable Steady under Time.

iii. Enable Absolute under Velocity Formulation.

b. In the Energy dialog box, enable the Energy option (if it is not already enabled).

ON

c.

In the Viscous Model dialog box, enable the Laminar option (if it is not already enabled).

Edit...

d. In the Species Model dialog box, configure the following settings:

Edit...

i.

Enable the Species Transport option.

ii.

Enable the Volumetric option under Reactions (see Enabling Species Transport and Reactions

and Choosing the Mixture Material in the Fluent User's Guide (p. ) for details).

iii. From the Mixture Material drop-down list, select an appropriate mixture material or create your

own mixture material from mixture-template as described in Enabling Species Transport and

Reactions and Choosing the Mixture Material in the Fluent User's Guide (p. ). If you consider

H2/CO electrochemistry, ensure that your mixture material include H2, CO and CO2.

iv. Disable the Inlet Diffusion option under Options (see Diffusion at Inlets in the Fluent Theory Guide).

v.

Enable the Diffusion Energy Source option under Options (see Treatment of Species Transport

in the Energy Equation in the Fluent Theory Guide).

vi. Enable the Full Multicomponent Diffusion option under Options (see Mass Diffusion in Laminar

Flows in the Fluent Theory Guide).

vii. Enable the Thermal Diffusion option under Options (see Mass Diffusion in Laminar Flows in the

e. Enable the SOFC Model model and set the parameters for the SOFC with unresolved electrolyte

model:

Edit...

i.

In the Model Parameters tab, set the Current Under-Relaxation Factor to a value of either .

or ..

ii.

Under Model Options, select the appropriate SOFC model options.

iii. Set the Electrical and Electrolyte Parameters according to your problem specification.

iv. Select the Enable Surface Energy Source option, the Enable Species Sources option, and the

Disable CO Electrochemistry option.

If the electrolyte resistivity changes as a function of temperature, then turn on the Enable

Electrolyte Conductivity Submodel

Interface Current Density (

)

UDM-

Nernst Potential (Volts)

UDM-

)

UDM-

UDM-

Activation Overpotentail (Volts)

UDM-

Volumetric Ohmic Source (

)

UDM-

x Component of the Current Density (

)

UDM-

y Component of the Current Density (

)

UDM-

z Component of the Current Density (

)

UDM-

Electrolyte Voltage Jump

UDM-

Electrolyte Resistivity (Ohm-m)

UDM-

UDM-

Anode Activation

UDM-

Cathode Activation

UDM-

Electrochemical Source (

)

UDM-

Magnitude of Current Density (

)

UDM-

Note that UDM- and UDM- are the linearized values that ANSYS Fluent uses to solve the

potential field and electrochemical coupling. They are necessary to the calculations but do

not contain any real physical meaning.

Note that UDM- and UDM- contain the disaggregated activation polarizations at the

anode and cathode.

f.

In the Electrochemistry tab, set the electrochemistry parameters.

i.

Enter values for the Constant Exchange Current Densities for the anode and the cathode.These

are the  values in the Butler-Volmer equation (Equation .) for the anodic and cathodic reac-

tions. By default, the Anode Exchange Current Density is set to  Amps and the Cathode

Exchange Current Density is set to  Amps.

ii.

Enter values for the Mole Fraction Reference Values.

These are the species concentrations at which the exchange current densities were taken

(Equation .-Equation . ). These are used to adjust the  values of reactant species

that are depleted. By default, the H2 Reference Value is set to . moles/moles, the O2

Reference Value is set to . moles/moles, and the H2O Reference Value is set to .

moles/moles.

iii. Enter values for the Stoichiometric Exponents by setting values for the H2 Exponent, the H20

Exponent, and the O2 Exponent (defaulted to . ).These are the stoichiometric factors in the

electrochemical reaction equation.They are used as exponents as part of the  scaling (Equa-

tion . and Equation ..

iv. Enter values for the Butler-Volmer Transfer Coefficients by setting values for the Anodic

Transfer Coefficient (

in Equation .) and the Cathode Transfer Coefficient (

in Equa-

tion .) for both the anode reaction and the cathode reaction (defaulted to . ).These are

the alpha values in the Butler-Volmer equation (Equation . ).They represent the forward and

backward rates of reaction at both the anode and cathode.

v.

Enter values for the Temperature Dependent Exchange Current Density by turning on the Enable

Temperature Dependent I_0 option and setting values for A and B (Equation . (p. )).These

two coefficients allow the  for the cathode to vary as a function of temperature.

g. In the Electrode and Tortuosity tab, set the anode and cathode interface components and set the

tortuosity parameters for the SOFC With Unresolved Electrolyte Model.

i.

Under Anode Electrolyte, select a zone in the Zone(s) list and enable Anode Interface if it is ap-

plicable.

ii.

Do the same for Cathode Electrolyte and Tortuosity Zone.

h. In the Electric Field tab, set the parameters for the electric field model.

i.

Select up to  conductive regions.

ii.

Select up to  contact surfaces.

i.

ii.

iii. Select a voltage tap surface.

iv. Select a current tap surface.

a.

Create or re-define new solid materials as appropriate for the anode, the cathode, and the electrolyte

according to your problem specification.

Important

Note that although the ANSYS Fluent SOFC With Unresolved Electrolyte Model does

support the shell conduction model that you use to take into account the transversal

conductive heat inside the electrolyte material, it does not currently support a similarly

transversal conduction of electric current inside the electrolyte.

b. Edit the mixture-template mixture material.

Setup →

i.

In the Create/Edit Materials dialog box, click Fluent Database... to open the Fluent Database

Materials dialog box.

ii.

In the Fluent Database Materials dialog box, make a copy of the h2 fluid material.

iii. In the Create/Edit Materials dialog box, change the Material Type to mixture and click Edit...

for the Mixture Species.

iv. In the Species dialog box, arrange the materials under Selected Species in the following order:

h2o, o2, h2, and n2. (The species ordering is not important as long as n2 is the last species.)

v.

In the Create/Edit Materials dialog box, change the Thermal Conductivity and the Viscosity to

ideal-gas-mixing-law.

vi. Change the Mass Diffusivity to user-defined and select diffusivity::sofc as the corresponding

user-defined function.

vii. Change the UDS Diffusivity to user-defined and select E_Conductivity::sofc as the corresponding

viii.Retain the default values for the other parameters and click Change/Create.

Setup →

Retain the default values.

Setup →

Define the conditions at the anode, the cathode, the interface between the anode and current

collector, the interface between the cathode and the current collector, the anode inlet, and the

cathode inlet boundaries according to your problem specification.

Note that sources only need to be hooked to the mass, species, and energy equation in a single

fluid zone in order for the ANSYS Fluent SOFC With Unresolved Electrolyte Model to function

properly (but can be hooked to all zones if you so choose). ANSYS Fluent does not rely on cell or

thread referencing in the sources in order to cover the solution domain.

. Set the multigrid control parameters.

Advanced...

a.

In the Multigrid tab of the Advanced Solution Controls dialog box, set the cycle type for h2, h2o,

and o2 to V-cycle. For serial calculations, set the cycle type for Energy and User-defined Scalar- to

W-cycle or F-cycle. For parallel calculations, select the F-cycle option for both.

b. Set the Max Cycles to .

c.

Retain the default values for the rest of the parameters.

. Define the convergence criteria.

Edit...

In the Residual Monitors dialog box, set the Convergence Criterion for all equations to 1e-.

Solution →

Solution →

Retain the default values for all parameters.

The current density in UDM- is a conservative flux of electricity (

). Performing an area integral

over the electrolyte surface will sum to the total current ( ). That value is computed at the electrolyte

faces during the electric field solution. The values in UDM- through UDM- contain cell-centered

values of the current density vector. These are not, and cannot be, conservative, so depending on the

material conductivity and the geometric configuration, these can sometimes unavoidably produce

values that do not match the UDM values. The same issues exist when interpolating velocity values

to obtain the mass fluxes.

Note that, by default, the ANSYS Fluent SOFC With Unresolved Electrolyte Model defines a single user-

defined scalar:

UDS-

Note

CFD-Post.

... Setting the Parameters for the SOFC With Unresolved Electrolyte

Model

You can specify the general settings for the SOFC With Unresolved Electrolyte Model using the Model

Parameters tab in the SOFC Model dialog box.

Figure . : The Model Parameters Tab in the SOFC Model Dialog Box

From this tab, you can set the various parameters for the SOFC With Unresolved Electrolyte Model

such as total system current, electrolyte thickness, electrolyte resistivity, and so on.

The Enable Electrolyte Conductivity Submodel option allows the ionic conductivity (or resistivity)

of the electrolyte to change as a function of temperature. At the moment, there is one correlation that

provides ionic conductivity (or resistivity) of the electrolyte as function of temperature.

(.)

Important

Note that this is valid only for temperatures ranging from  K to  K.

By turning off the Enable Surface Energy Source option, ANSYS Fluent excludes the heat addition

due to electrochemistry and all the reversible processes. This option should be turned on at all times.

The Enable Volumetric Energy Source option includes the ohmic heating throughout the electrically

conducting zones. You should keep this option turned off (to avoid slowing the convergence rates)

until a certain rate of convergence for the potential field has been achieved, at which point, you should

turn the option on manually. Note that this option is important so that the solution can account for

the effects of the internal Ohmic heating.

The Disable CO Electrochemistry is enabled if there is carbon monoxide (CO) in the fuel line and if

you do not want to include the CO in the electrochemistry.

Since the calculations are very sensitive to large current fluctuations early in the solution process, it is

recommended that you use . or . for the Current Under-Relaxation Factor for a more effective

solution.

solution.

The leakage current is the total amount of current due to the leakage of oxidizer to the fuel side

(through the electrolyte) and the electric current across the electrolyte due to any short circuit. You

can specify a value for the leakage current under Leakage Current Density.

If the leakage current density is temperature-dependent, you can specify your own temperature-de-

pendent implementation of the leakage current density by performing the following steps:

. Make the required changes to Leakage_Current_Density (real T) which is a real function in

the user-modifiable source code, constit.c.

. Compile constit.c and make your own sofc UDF library.

For more information, see Compiling the Customized Solid Oxide Fuel Cell With Unresolved Elec-

trolyte Source Code (p. ).

The Converge to Specified System Voltage is used when you want to specify a system voltage instead

of system current as an input.

The Set Individual Electrical Boundary Condition from Boundary Conditions Task Page option,

when enabled, allows you to directly specify the current density or voltage for each individual current-

collecting boundary using the ANSYS Fluent Boundary Conditions task page. This allows you to apply

multiple current types or multiple voltage types (either constant or variable) to your boundary conditions.

You can specify electrochemistry settings for the SOFC With Unresolved Electrolyte Model using the

Electrochemistry tab in the SOFC Model dialog box.

Figure . : The Electrochemistry Tab in the SOFC Model Dialog Box

In the Electrochemistry tab, you can set the anode and cathode exchange current density, the anode

and cathode mole fraction reference values, the concentration exponents, the Butler-Volmer transfer

coefficients, and the temperature-dependent exchange current density.

You can specify a value for the exchange current density at the anode (the default value is

) using the Anode Exchange Current Density field. Likewise, you can specify a value for

the exchange current density at the cathode (the default value is

) using the Cathode

Exchange Current Density field.

You can also specify Mole Fraction Reference Values (Equation .-Equation .) for the fuel

cell reactants in the Electrochemistry tab. By default, the reference value for

is ., the reference

value for

is ., and the reference value for

is ..

The Butler-Volmer transfer coefficients can be set in the Electrochemistry tab as well. These coefficients

are the

and

from Equation . for both the anode and the cathode reactions.

(.)

Remember that  has anodic and cathodic values at both the cathode and the anode. By default, the

value of  is set to . because of the nearly universal assumption that there is a symmetric balance

between the forward and backward reactions. In most cases, these default values will be sufficient.

If you find yourself changing the Butler-Volmer transfer coefficients, or if you have some other rate-

limiting reaction in your fuel cell simulation, you may also want to consider changing the exponents

for the stoichiometric coefficients for the fuel cell reactants. These exponents can be specified in the

Electrochemistry tab. By default, the exponent values for

,

, and

are ..

The Enable Temperature Dependant I_0 option allows the exchange current density to change as

a function of temperature in an exponential fashion

(.)

where you can provide the values for the constants  and .

You can apply specific settings for both your anode and your cathode interfaces as well as set tortuosity

parameters using the ANSYS Fluent SOFC With Unresolved Electrolyte Model through the Electrolyte

and Tortuosity tab in the SOFC Model dialog box.

Figure . : The Electrolyte and Tortuosity Tab in the SOFC Model Dialog Box

. Set up the anode electrode-electrolyte interface.

a.

Enable the Anode Interface option.

b. Select the surface that represents the anode electrode interface with the electrolyte from the corres-

ponding Zone(s) list

c.

. In a similar manner, you can set up the cathode electrode-electrolyte interface.

. Set up the tortuosity parameters.

a.

Select the Enable Tortuosity option.

b. Select the appropriate zone from the corresponding Zone(s) list

c.

As required, assign tortuosity values to any porous zones in your simulation. In a porous zone, the

mass diffusion coefficient is reduced as follows due to the porosity effect:

(.)

There typically are no standard means of measuring tortuosity as it must be either measured

(.)

experimentally or tuned to match other experimental data. Tortuosity value may typically be

in the range of  to , although you can use much higher values.

d. Click Apply.

You can do this for as many zones as you need. When you are finished setting up the anode interface,

click the OK button.

You can set up the details of the electric field model using the Electric Field tab in the SOFC Model

Figure . : The Electric Field Tab in the SOFC Model Dialog Box

Here, you can designate conductive regions and specify their conductivity, assign boundaries to be

contact surfaces and specify the contact resistances, as well as specify which surfaces are grounded

and which surfaces exhibit a current.

The Voltage Tap Surface is the surface that is grounded (that is,

). The Current Tap Surface is

the surface that current is being drawn from (that is,  is assigned a value).

... User-Accessible Functions for the Solid Oxide Fuel Cell With Unre-

solved Electrolyte Model

You can directly incorporate your own formulations and data for the properties of the solid oxide fuel

cell model using the constit.c source code file.

The following listing represents a description of the contents of the constit.c source code file:

real Nernst (real sp_a[], real sp_c[], real P_a, real P_c, real T_a, real

T_c, real *DNDY)

Returns the Nernst potential using Equation ..

real Activation (real Y[], real P, real T, real i, real i_0, real alpha_a,

real alpha_b, int species, real *dA_di)

Returns the activation overpotential by solving Equation ..

real Resistivity (real T)

Returns the electrolyte resistance (either a constant value, or computed using Equation . (p. )).

real Leakage_Current_Density(realT)

Returns the leakage current density specified in the SOFC Model dialog box and can be overwritten as

a function of temperature.

real Solve_Butler_Volmer_NR (real i, real i0, real A, real B, real *detadi);

real CONDUCTIVITY_CELL(cell_t c, Thread *t)

Returns the cell conductivity value used in the Electric Field tab of the SOFC Model dialog box.This

function can be overwritten to look up the conductive zone group ID ( through ). A conditional statement

allows you to perform various tasks for respective conductive zones. For non-conductive zones, this

function returns a value of .

real CONTACT_RESIST_FACE (face_t f, Thread *t)

Returns the contact resistance value used in the Electric Field tab of the SOFC Model dialog box.This

function can be overwritten to look up the contact resistance group ID ( through ). A conditional

statement allows you to perform various tasks for respective contact resistance surfaces. For non-contact

resistance surfaces, this function returns a value of .

real h2_co_split_func(cell_t c_an, Thread *t_an)

/

split factor defined in Equation ..This can be overwritten as needed to define

your own split factor.

For more information, see Compiling the Customized Solid Oxide Fuel Cell With Unresolved Electrolyte

Source Code (p. ).

.... Compiling the Customized Solid Oxide Fuel Cell With Unresolved Electrolyte Source Code

.... Compiling the Customized Solid Oxide Fuel Cell With Unresolved Electrolyte

Source Code

This section includes instructions on how to compile a customized Solid Oxide Fuel Cell With Unre-

solved Electrolyte user-defined module.

Important

You will first want to use a local copy of the sofc directory in the addons directory before you re-

compile the Solid Oxide Fuel Cell With Unresolved Electrolyte module.

. Make a local copy of the sofc directory. Do not create a symbolic link.

Important

by ANSYS Fluent: for example, sofc.

. Change directories to the sofc/src directory.

. Make changes to the constit.c file.

Solid Oxide Fuel Cell With Unresolved Electrolyte module.

. Change directories to the sofc/ directory.

. Make a directory.

mkdir -p /home/sample

cp -RH [ansys_inc/v195/fluent]/fluent19../addons/sofc

/home/sample/sofc

. Using a text editor, make the appropriate changes to the constit.c file located in

/home/sample/sofc/src/constit.c

cd /home/sample/sofc

. Make a local copy of the sofc folder. Do not create a shortcut.

. Enter the sofc\src folder.

. Return to the sofc folder.

Chapter : Modeling Magnetohydrodynamics

The ANSYS Fluent Magnetohydrodynamics (MHD) Module Chapter tells you what you need to know to

model magnetohydrodynamics with ANSYS Fluent. Additional information about the model is provided

.. Implementation

.. Using the ANSYS Fluent MHD Module

.. Guidelines For Using the ANSYS Fluent MHD Model

.. Definitions of the Magnetic Field

.. External Magnetic Field Data Format

Magnetohydrodynamics refers to the interaction between an applied electromagnetic field and a

flowing, electrically-conductive fluid. The ANSYS Fluent MHD model enables you to analyze the behavior

of electrically conducting fluid flow under the influence of constant (DC) or oscillating (AC) electromag-

netic fields. The externally-imposed magnetic field may be generated either by selecting simple built-

in functions or by importing a user-supplied data file. For multiphase flows, the MHD model is compatible

with both the discrete phase model (DPM), the volume-of-fluid (VOF) and Eulerian Multiphase in ANSYS

Fluent, including the effects of a discrete phase on the electrical conductivity of the mixture.

This chapter describes the ANSYS Fluent MHD model. Modeling Magnetohydrodynamics provides the-

oretical background information. Implementation (p. ) summarizes the UDF-based software imple-

mentation. Instructions for getting started with the model are provided in Using the ANSYS Fluent MHD

Module (p. ). Guidelines For Using the ANSYS Fluent MHD Model (p. ) provides a condensed

overview on how to use the MHD model, while Definitions of the Magnetic Field (p. ) contains

definitions for the magnetic field, External Magnetic Field Data Format (p. ) describes the external

magnetic field data format, and Magnetohydrodynamics Text Commands  lists the text commands in

the MHD model.

The MHD model is implemented using user-defined functions (UDF) as an ANSYS Fluent add-on module,

which is loaded into ANSYS Fluent at run time. The model is accessed through a number of UDF schemes.

The magnetic induction equation given by Equation . or Equation . and the electric potential

equation given by Equation . are solved through user-defined scalar (UDS) transport equations.

Other model-related variables such as the external magnetic field data, current density, Lorentz force

and Joule heat are stored as user-defined memory (UDM) variables. The MHD model setup and parameters

are entered using the MHD Model graphical user interface (GUI) dialog box and a set of text user interface

(TUI) commands described in Using the ANSYS Fluent MHD Module (p. ). Detailed information can

be found in the following sections:

... Solving Magnetic Induction and Electric Potential Equations

... Calculation of MHD Variables

... MHD Interaction with Fluid Flows

... MHD Interaction with Discrete Phase Model

... General User-Defined Functions

The magnetic induction equation and the electric potential equations are solved through user-defined

scalar transport equations. For the magnetic induction equation a set of  or  scalar equations are

solved, each representing a Cartesian component of the induced magnetic field vector in a 2D or 3D

case. For the electric potential equation a single scalar equation is solved.

The convection and the diffusion terms of the scalar equations are defined using user functions

DEFINE_UDS_FLUX(mhd_flux, ..., ns) and DEFINE_DIFFUSIVITY (mhd_ magnet-

ic_diffusivity, ..., ns) respectively. The user-defined scalar equation is identified by the

scalar index ns.

The source terms to the induction equations and the potential equation are implemented using user

function DEFINE_SOURCE(mhd_mag_source, ..., eqn) and DEFINE_SOURCE

(mhd_phi_source, ..., eqn) respectively, where eqn identifies the scalar equations.

For transient cases, the additional unsteady source term is introduced through the user function

DEFINE_UDS_UNSTEADY(mhd_unsteady_source, ..., ns), where ns identifies the scalar

being solved.

The induction and potential equations can also be solved in solid zones, in which case the fluid velocity

terms in the equations are not considered. For multiphase flows, the MHD equations are solved in the

mixture domain only.

The wall boundary conditions are implemented through user profile functions (DEFINE_PRO-

FILE(mhd_bc_...), and are applied to the Cartesian components of the induced magnetic field

vector or to the electric potential. For external wall boundaries, three types of boundary conditions

(electrically insulating, conducting, and "thin wall"), can be applied. The ’thin wall’ type boundary refers

to an external wall where a 1D magnetic or electric potential diffusion normal to the boundary is as-

sumed, and the wall material and the thickness are specified for the boundary. For internal wall

boundaries, that is the boundaries between fluid/solid or solid/solid zones, a coupled boundary condition

is applied.

Apart from the Cartesian components of the magnetic field vectors and the electric potential function,

which are stored as user-defined scalars, other MHD-related variables include the induced electric

current density vector, induced electric field vector, the Lorentz force vector and Joule heat. These

variables are stored in user-defined memory locations. Updating of MHD variables is accessed through

the user function DEFINE_ADJUST(mhd_adjust,...). The variables are updated at the start of

each iteration using the solved induced magnetic field from the previous iteration.

Additional source terms due to the magnetic induction are added to the flow momentum and energy

equations as user defined source terms. For the momentum equation, user function

DEFINE_SOURCE(mhd_mom_source, ..., eqn) is used to introduce the Lorentz force to the

equation, where eqn identifies the Cartesian component of the fluid momentum. For the energy

Modeling Magnetohydrodynamics

equation, the additional source due to Joule heating is added through user function

DEFINE_SOURCE(mhd_energy_source,..., eqn), where eqn is the energy equation index.

In discrete phase modeling, the Lorentz force acting on charged particles is introduced through the

user function DEFINE_DPM_BODY_FORCE(mhd_dpm_force, ...). User function

DEFINE_DPM_SOURCE(mhd_dpm_source, ...) is used to update the volume fraction of the

discrete phase inside a fluid cell and the volume-weighted electric conductivity of the discrete phase.

Several general UDFs are used as part of the MHD model implementation.

DEFINE_INIT(mhd_init,...) is an initialization function called during the general case initialization

to set up the external magnetic field and initialize MHD model parameters and variables.

DEFINE_ADJUST(mhd_adjust,...) is called at the start of each iteration. It is used to adjust the

magnetic boundary conditions and update MHD related variables and properties.

This chapter provides basic instructions to install the magnetohydrodynamics (MHD) module and solve

MHD problems in ANSYS Fluent. It assumes that you are already familiar with standard ANSYS Fluent

Guidelines For Using the ANSYS Fluent MHD Model (p. ) also outlines the general procedure for using

the MHD model. This chapter describes the following:

... MHD Module Installation

... Loading the MHD Module

... MHD Model Setup

... MHD Solution and Postprocessing

The MHD module is provided as an add-on module with the standard ANSYS Fluent licensed software.

The module is installed in a directory called addons/mhd in your installation area. The MHD module

consists of a UDF library and a pre-compiled Scheme library, which must be loaded and activated before

calculations can be performed.

The MHD module is loaded into ANSYS Fluent through the text user interface (TUI). The module can

only be loaded when a valid ANSYS Fluent case file has been set or read. The text command to load

define → models → addon-module.

Using the ANSYS Fluent MHD Module

. None

. MHD Model

Select the MHD model by entering the module number . During the loading process a Scheme library

containing the graphical and text user interface, and a UDF library containing a set of user defined

functions are loaded into ANSYS Fluent. A message Addon Module: mhd...loaded! is displayed at the

end of the loading process.

The basic set up of the MHD model is performed automatically when the MHD module is loaded suc-

cessfully. The set up includes:

Selecting the default MHD method

Allocating the required number of user-defined scalars and memory locations naming of:

– User-defined scalars and memory locations

– All UDF Hooks for MHD initialization and adjustment

– MHD equation flux and unsteady terms

– Source terms for the MHD equations

– Additional source terms for the fluid momentum and energy equations

– Default MHD boundary conditions for external and internal boundaries

– A default set of model parameters

DPM related functions are also set, if the DPM option has been selected in the ANSYS Fluent case set up.

The MHD module set up is saved with the ANSYS Fluent case file. The module is loaded automatically

when the case file is subsequently read into ANSYS Fluent. Note that in the saved case file, the MHD

module is saved with the absolute path. Therefore, if the locations of the MHD module installation or

the saved case file are changed, ANSYS Fluent will not be able to load the module when the case file

is subsequently read.

To unload the previously saved MHD module library, open the UDF Library Manager dialog box

Parameters & Customization → User Defined Functions

Manage...

and reload the module as described above. Note that the previously saved MHD model setup and

parameters are preserved.

Following the loading of the MHD module, you can access the MHD Model dialog box using

Setup → Models → MHD Model

Edit...

or using the text command

define → models → mhd-model

Both the MHD Model dialog box and TUI commands are designed for the following tasks:

Enable/disable the MHD model.

Select the MHD method.

Apply an external magnetic field.

Set boundary conditions.

Set solution control parameters.

Operations of these tasks through the MHD Model dialog box are described in the following sections.

The set of MHD text commands are listed in Magnetohydrodynamics Text Commands .

.... Enabling the MHD Model

.... Selecting an MHD Method

.... Applying an External Magnetic Field

.... Setting Up Boundary Conditions

.... Solution Controls

If the MHD model is not enabled after the MHD module is loaded for the first time, you can enable

it by selecting Enable MHD in the MHD Model dialog box, shown in Figure . : Enabling the MHD

Model Dialog Box (p. ). The dialog box expands to its full size when the model is enabled, as shown

in Figure . : The MHD Model Dialog Box (p. ).

Figure . : Enabling the MHD Model Dialog Box

Figure . : The MHD Model Dialog Box

The method used for MHD calculation can be selected under MHD Method in the MHD Model dialog

box. The two methods, Magnetic Induction and Electrical Potential, are described in Magnetic In-

duction Method and Electric Potential Method,

For the Magnetic Induction method,  or  user-defined scalars are allocated for the solution of the

induced magnetic field in 2D or 3D cases. The scalars are listed as B_x, B_y and B_z representing the

Cartesian components of the induced magnetic field vector. The unit for the scalar is Tesla.

For the Electrical Potential method,  user-defined scalar is solved for the electric potential field. The

scalar is listed as

and has the unit of Volt.

Table . : User-Defined Scalars in MHD Model (p. ) lists the user-defined scalars used by the two

methods.

Table . : User-Defined Scalars in MHD Model

Unit

Name

Scalar

Method

X component of induced magnetic field (

)

Tesla

B_x

Scalar-

Induction

Y component of induced magnetic field (

)

Tesla

B_y

Scalar-

Unit

Name

Scalar

Method

Z component of induced magnetic field (

)

Tesla

B_z

Scalar- (-D)

Electric potential ( )

Volt

Phi

Scalar-

Potential

Application of an external magnetic field to the computation domain is done under the External

Field B0 tab in the MHD Model dialog box, as shown in Figure . : The MHD Model Dialog Box for

Patching an External Magnetic Field (p. ). Two B0 Input Options are available for setting up the

external magnetic field. One option is to Patch the computational domain with a constant (DC Field)

and/or varying (AC Field) type. The other option is to Import the field data from a magnetic data

file that you provide.

With the Patch option enabled, the AC field can be expressed as a function of time (specified by

Frequency), and space (specified by wavelength, propagation direction and initial phase offset). The

space components are set under the B0 Component, as in Figure . : The MHD Model Dialog Box

for Patching an External Magnetic Field (p. ).

Figure . : The MHD Model Dialog Box for Patching an External Magnetic Field

You can also specify a Moving Field with a wave form that is either a sinusoidal or a square wave

function (Figure . : The MHD Model Dialog Box for Specifying a Moving Field (p. )). Definitions

for the sinusoidal and square wave forms of patched magnetic fields are provided in Definitions of

the Magnetic Field (p. ).

Figure . : The MHD Model Dialog Box for Specifying a Moving Field

Selecting Import under the B0 Input Option in the MHD Model dialog box, as seen in Figure . : The

MHD Model Dialog Box for Importing an External Magnetic Field (p. ), will result in the import of

magnetic field data. The data filename can be entered in the B0 Data File Name field, or selected

from your computer file system using the Browse... button. Magnetic data can also be generated

using a third-party program such as MAGNA. The required format of the magnetic field data file is

given in External Magnetic Field Data Format (p. ).

When using the Import option, the B0 Data Media is either set to Non-Conducting or Conducting,

depending on the assumptions used in generating the magnetic field data. (These choices correspond

to “Case ” and “Case ”, respectively, as discussed in Magnetic Induction Method.)

Figure . : The MHD Model Dialog Box for Importing an External Magnetic Field

The Field Type is determined by the field data from the data file. The choice of either the DC Field

or the AC Field option in the dialog box is irrelevant if the import data is either DC or AC. However,

selection of both options indicates that data of both field types are to be imported from the data

file, and superimposed together to provide the final external field data. Make sure that the data file

contains two sections for the required data. See External Magnetic Field Data Format (p. ) for details

on data file with two data sections.

The Apply External Field... button opens the Apply External B0 Field dialog box as shown in Fig-

ure . : Apply External B0 Field Dialog Box (p. ). To apply the external field data to zones or regions

in the computational domain, select the zone names or register names of marked regions from the

dialog box and click the Apply button.

The Reset External Field button sets the external magnetic field variable to zero.

Figure . : Apply External B0 Field Dialog Box

Boundary conditions related to MHD calculations are set under the Boundary Condition tab in the

MHD Model dialog box. Boundary conditions can be set to cell zones and wall boundaries.

For cell zones, only the associated material can be changed and its properties modified. Figure . : Cell

Boundary Condition Setup (p. ) shows the dialog box for cell zone boundary condition setup. The

cell zone material can be selected from the Material Name drop-down list.

Figure . : Cell Boundary Condition Setup

Note that the materials available in the list are set in the general ANSYS Fluent case set up. Refer to

the ANSYS Fluent User Guide for details on adding materials to an ANSYS Fluent case. The properties

of the selected material can be modified in the Boundary Condition tab by clicking Edit... to the

right of the material name. This opens the Edit Material dialog box, as shown in Figure . : Editing

Material Properties within Boundary Condition Setup (p. ). The material properties that may be

modified include the electrical conductivity and magnetic permeability. The material electrical con-

ductivity can be set as constant, a function of temperature in forms of piecewise-linear, piecewise-

polynomial or polynomial, or as a user-defined function. The material magnetic permeability can only

be set as a constant.

Figure . : Editing Material Properties within Boundary Condition Setup

For wall boundaries, the boundary condition can be set as an Insulating Wall, Conducting Wall,

Coupled Wall or Thin Wall. The dialog box for wall boundary condition set up is shown in Fig-

ure . : Wall Boundary Condition Setup (p. ).

Figure . : Wall Boundary Condition Setup

The insulating wall is used for boundaries where there is no electric current going through the boundary.

The conducting wall is used for boundaries that are perfect conductors.

The coupled wall should be used for wall boundaries between solid/solid or solid/fluid zones where the

MHD equations are solved.

The thin wall type boundary can be used for external wall that has a finite electrical conductivity.

For conducting walls and thin wall boundaries, the wall material can be selected from the Material

Name drop-down list, and its properties modified through the Edit Material dialog box. A wall

thickness must be specified for thin wall type boundaries.

If the Electric Potential method is selected, the conducting wall boundary is specified by either of

Voltage or Current Density at the boundary, as shown in Figure . : Conducting Wall Boundary

Conditions in Electrical Potential Method (p. ).

Figure . : Conducting Wall Boundary Conditions in Electrical Potential Method

Under the Solution Control tab in the MHD Model dialog box, Figure . : Solution Control Tab in

the MHD Model Dialog Box (p. ), a number of parameters can be set that control the solution

process in an MHD calculation. The MHD model can be initialized using the Initialize MHD button.

When the DPM model is enabled in the ANSYS Fluent case set up, the related variables used in the

MHD model can be initialized using the Initialize DPM button.

Figure . : Solution Control Tab in the MHD Model Dialog Box

You have the option to enable or disable the Solve MHD Equation. When the Solve MHD Equation

is enabled, you have the choice to Include Lorentz Force and/or Include Joule Heating in the

solution of flow momentum and energy equations. The under-relaxation factor for the MHD equations

can also be set.

The strength of the imposed external magnetic field can be adjusted by specifying and applying scale

factors to the external DC and/or AC magnetic field data.

The following sections describe the solution and postprocessing steps for the MHD model:

.... MHD Model Initialization

.... Iteration

.... Postprocessing

Initialization of the MHD model involves setting the externally-imposed magnetic field and initializing

all MHD related user-defined scalars and memory variables.

When an ANSYS Fluent case is initialized, all user-defined scalar and memory variables are set to zero.

The external magnetic field data is set from the External Field B0 tab in the MHD Model dialog box.

The Initialize MHD button under the Solution Control tab can be used to initialize the model during

an ANSYS Fluent solution process. It is used when MHD effects are added to a fully or partially solved

flow field, or when the model parameters are changed during an MHD calculation. It only clears the

scalar variables and most of the memory locations used in the MHD model, the memory variables for

the external magnetic field data are preserved.

It is often an effective strategy to begin your MHD calculations using a previously-converged flow

field solution. With this approach, the induction equations themselves are generally easy to converge.

The under-relaxation factors for these equations can be set to .

., although for very strong

magnetic fields, smaller values may be needed. For the electric potential equation, the convergence

is generally slow. However, the under-relaxation value for this equation should not be set to . As

additional source terms are added to the momentum and energy equations, the under-relaxation

factors for these equations should generally be reduced to improve the rate of convergence. In case

of convergence difficulties, another helpful strategy is to use the B0 Scale Factor in the Solution

Control tab (Figure . : The MHD Model Dialog Box (p. )). This will gradually increase the MHD

effect to its actual magnitude through a series of restarts. When the strength of the externally imposed

magnetic field is strong, it is advisable to start the calculation with a reduced strength external field

by applying a small scale factor. When the calculation is approaching convergence the scale factor

can be increased gradually until the required external field strength is reached.

You can use the standard postprocessing facilities of ANSYS Fluent to display the MHD calculation

results.

Contours of MHD variables can be displayed using

Edit...

The MHD variables can be selected from the variable list.

Vectors of MHD variables, such as the magnetic field vector and current density vector, can be displayed

using

Edit...

The vector fields of the MHD variables are listed in the Vectors of drop-down list in the Vectors

dialog box. Table . : MHD Vectors (p. ) lists the MHD related vector fields.

Table . : MHD Vectors

Unit

Name

Induced magnetic field vector

Tesla

Induced- -Field

Applied external magnetic field vector

Tesla

External- -Field

Induced current density field vector

Current-Density

Unit

Name

Electric field density vector

V/m

Electric-Field

Lorentz force vector

Lorentz-Force

Note

Note

CFD-Post.

Many MHD applications involve the simultaneous use of other advanced ANSYS Fluent capabilities

such as solidification, free surface modeling with the volume of fluid (VOF) approach, DPM, Eulerian

multiphase, and so on. You should consult the latest ANSYS Fluent documentation for the limitations

that apply to those features. In addition, you should be aware of the following limitations of the MHD

capability.

As explained in Modeling Magnetohydrodynamics, the MHD module assumes a sufficiently conductive

fluid so that the charge density and displacement current terms in Maxwell’s equations can be neglected.

For marginally conductive fluids, this assumption may not be valid. More information about this simplific-

ation is available in the bibliography.

For electromagnetic material properties, only constant isotropic models are available. Multiphase volume

fractions are not dependent on temperature, species concentration, or field strength. However, sufficiently

strong magnetic fields can cause the constant-permeability assumption to become invalid.

You must specify the applied magnetic field directly.The alternative specification of an imposed electrical

current is not supported.

In the case of alternating-current (AC) magnetic fields, the capability has been designed for relatively low

frequencies; explicit temporal resolution of each cycle is required. Although not a fundamental limitation,

the computational expense of simulating high-frequency effects may become excessive due to small required

time step size.Time-averaging methods to incorporate high-frequency MHD effects have not been imple-

mented.

This section provides a basic outline for installing the magnetohydrodynamics (MHD) module and

solving MHD problems in ANSYS Fluent.

... Installing the MHD Module

Guidelines For Using the ANSYS Fluent MHD Model

... An Overview of Using the MHD Module

Important

While Using the ANSYS Fluent MHD Module (p. ) covers much of the same material in

greater detail, this section presents a set of guidelines for solving typical MHD problems with

ANSYS Fluent, with occasional references to Using the ANSYS Fluent MHD Module (p. )

where more information can be found.

Before using the MHD module, you first need to install the necessary files onto your computer. These

files are provided with your standard installation of ANSYS Fluent. They can be found in your installation

area in a directory called addons/mhd. The MHD module is loaded into ANSYS Fluent through the

text user interface (TUI)

only after a valid ANSYS Fluent case file has been set or read.

Once the MHD model is installed, beneath the mhd directory there are two subdirectories: a lib dir-

ectory, and a directory corresponding to your specific architecture, ntx86 for example. The lib dir-

ectory holds a Scheme code called addon.bin that contains the MHD module graphical interface.

The specific architecture directory, ntx86 for example, contains the following subdirectories that hold

various ANSYS Fluent files:

2d   2ddp   3d   3ddp

2d_host  2ddp_host  3d_host  3ddp_host

2d_node  2ddp_node  3d_node  3ddp_node

To use the MHD module in an ANSYS Fluent simulation, follow the general guidelines:

To begin modeling your MHD simulation, you need to start an appropriate ANSYS Fluent session.

Choose from either the 2D, 3D, Double Precision, or the parallel version of ANSYS Fluent.

. Read in a mesh file or a case file.

You can have ANSYS Fluent read in your mesh file, a previously saved non-MHD case file, or a

previously saved MHD case file.

Important

Note that if you read in a new mesh file, you need to perform the appropriate mesh

check and mesh scale procedures.

. Load the MHD module.

The MHD module is loaded into ANSYS Fluent using the text command

and entering the corresponding module number (Loading the MHD Module (p. )).

. Set up the MHD model.

The MHD Model dialog box is accessed using the graphical user interface (GUI):

Edit...

it by clicking the Enable MHD button, which will display the expanded dialog box (Enabling the

MHD Model (p. )).

. Select an MHD method.

The method used for the MHD calculation can be selected under MHD Method. The two methods

are

are

Magnetic Induction (Magnetic Induction Method)

Electrical Potential (Electric Potential Method)

. Apply an external magnetic field.

This is done by entering values for the B0 components in the External Field B0 tab. B0 input options

can either be

Patched, or

Imported

The Field Type will either be the DC Field or the AC Field. The Field Type is determined by the

field data from the data file. Refer to Applying an External Magnetic Field (p. ) for details on

applying an external magnetic field.

. Set up the boundary conditions.

Under the Boundary Condition tab, cell zones and wall boundaries can be selected as well as the

corresponding zone type.

Cell zone materials are selected from the Material Name drop-down list. The properties of the se-

lected material can be modified by clicking on the Edit... button to the right of the material name.

Note that the materials available in the list are set in the general ANSYS Fluent case setup.

Setup →

Materials

The material properties that may be modified include the electrical conductivity and magnetic

permeability.

Wall boundary conditions can be set as an Insulating Wall, Conducting Wall, Coupled Wall or

Thin Wall (see Setting Up Boundary Conditions (p. )).

. Set solution controls.

Under the Solution Control tab:

The MHD equation is enabled or disabled.

Lorentz force and Joule heat sources are enabled or disabled.

under-relaxation factors are set (reasonable under-relaxation factors for the MHD equations are .

. ).

. ).

Scale factors can be used to adjust the strength of the imposed external magnetic field. As the calculation

approaches convergence, the scale factor in the Solution Control tab can be increased gradually until

the required external field strength is reached (Solution Controls (p. )).

The MHD model is initialized (MHD Model Initialization (p. )).

. Run the ANSYS Fluent MHD simulation.

Solution →

Set the number of iterations. It is often an effective strategy to begin your MHD calculations using

a previously-converged flow field solution. With this approach, the induction equations themselves

are generally easy to converge. For more information, see Iteration (p. ).

. Process the solution data.

You can use the standard postprocessing facilities of ANSYS Fluent to display the results of an MHD

calculation. Contours of MHD variables can be displayed.

Edit...

The MHD variables can be selected from the variable list. Vectors of MHD variables, such as the

magnetic field vector and current density vector, can be displayed using custom vectors.

Edit...

For more information, see Postprocessing (p. ).

The sinusoidal form of the magnetic field is defined as:

(.)

where

is the mean vector,

is the amplitude vector,

is defined as the propagation vector,

is

the position vector of an arbitrary point.

,

and

are the ,

and  direction cosines

respectively. The quantities ,

, and

are the frequency, wavelength, and phase offset, respectively.

is

,

and

are the ,

, and

For a non-moving field, the propagation vector is zero.

The square form of the magnetic field is defined as:

(.)

The definition of the propagation vector is the same as for the sinusoidal form.

The external magnetic field data file is in text format and of the following structure:

...

The first line is an identification tag for the data file. The second line defines the number of data points

in the ,

and  directions. The next three lines define the ranges in ,

and  directions. The data

points are assumed to be evenly distributed along each direction. Line  defines the AC field flag and

frequency. When nAC = , the magnetic field is static. For AC field, nAC =  and Freq is the frequency

in Hz.

The rest of the data file contains the magnetic field data points. Each line defines the components of

the real and imaginary parts of the magnetic field vector on one data point. The data points are indexed

as:

(.)

The data is listed in the ascending order from  to , where  is the total number of data points given

by  =

.

For magnetic fields composed of both DC and AC fields, the entire file structure described above is re-

peated for the DC and AC parts. These two sections within the same file will be imported into ANSYS

Fluent and stored separately. The order of the DC and AC sections of the file is not important.

The imported data is interpreted as a snapshot of the applied magnetic field at an instant in time.

Complex form is used to accommodate oscillating/moving fields. Thus, using complex numbers, and

with reference to the quantities defined in Definitions of the Magnetic Field (p. ),

(.)

External Magnetic Field Data Format

For a DC field,

(.)

For an AC field,

(.)

and

(.)

Note that when the external magnetic field import option is used, the frequency,

, read from this file

supersedes the value specified in the GUI.

Chapter : Modeling Continuous Fibers

The continuous fiber model is provided as an add-on module with the standard ANSYS Fluent licensed

software.

Several fiber spinning techniques exist in industrial fiber production. The most common types are melt

spinning and dry spinning.

In melt spinning, the polymer is heated above its melting point and extruded in a liquid state through

nozzles into a vertical spinning chamber. The molten polymer is processed in an inert gas environment,

such as nitrogen, then extruded at high pressure and a constant rate into a cooler air stream, thus so-

lidifying the fiber filaments.

In dry spinning, the liquefaction of the polymer is obtained by dissolving it in a suitable solvent. This

technique often is applied to polymers that are destroyed thermally before reaching its melting point

or if the production process leads to a solvent/polymer mixture. In the spinning chamber, the solvent

vaporizes by drying with a hot air stream. The solidification ensures that the fiber is nearly free of solvent.

ANSYS Fluent’s continuous fiber model allows you to analyze the behavior of fiber flow, fiber properties,

and coupling between fibers and the surrounding fluid due to the strong interaction that exists between

the fibers and the surrounding gas.

This document describes the ANSYS Fluent Continuous Fiber model. Modeling Continuous Fibers

provides theoretical background information.

The procedure for setting up and solving fiber spinning flows is described in detail in this chapter. Only

the steps related to fiber modeling are shown here.

Important

Note that the continuous fiber model is available for the pressure-based solver, only.

For information about inputs related to other models used in conjunction with the fiber models, see

the appropriate sections for those models in the ANSYS Fluent User's Guide (p. ).

.. Installing the Continuous Fiber Module

.. Loading the Continuous Fiber Module

.. Getting Started With the Continuous Fiber Module

.. Fiber Models and Options

.. Fiber Material Properties

.. Defining Fibers

.. User-Defined Functions (UDFs) for the Continuous Fiber Model

.. Fiber Model Solution Controls

.. Postprocessing for the Continuous Fibers

software. The module is installed with the standard installation of ANSYS Fluent in a directory called

addons/fiber in your installation area. The continuous fiber module consists of a UDF library and a

pre-compiled Scheme library, which must be loaded and activated before calculations can be performed.

The continuous fiber module is loaded into ANSYS Fluent through the text user interface (TUI). The

module can be loaded only when a valid ANSYS Fluent case file has been set or read. The text command

to load the module is

. None

. MHD Model

. MSMD Battery Module

Select the continuous fiber model by entering the module number . During the loading process a

Scheme library containing the graphical and text user interface, and a UDF library containing a set of

user-defined functions (UDFs) are loaded into ANSYS Fluent.

During this process, you will be asked the question

Preset all fiber model specific UDF hooks? [no]

If you answer yes the standard fiber source term UDFs will be assigned to all fluid zones in your case,

and a message will be reported to the console window confirming this:

Assigning standard fiber source terms to all fluid zones.

If you answer no to presetting source term UDFs to all fluid zones in the domain, then three options

will be available to you when setting up source terms for fluid zones in your fiber model: no source,

constant source, or UDF source. Note that it is your responsibility to specify the rest of the settings for

a proper fiber simulation. See Source Term UDF Setup (p. ) for details.

If you are loading an existing case file then you should answer the question with no. Otherwise, your

saved source term settings will be replaced by a UDF.

If a mixture material has been defined, then you will be asked an additional question

Preset mass exchange source terms hooks? [no]

Modeling Continuous Fibers

If you intend to conduct a dry spinning simulation, then you should reply yes.

During the loading process the UDF library for the continuous fiber module is loaded in ANSYS Fluent.

This is reported to the console (see below). The UDF library also becomes visible as a new entry in the

UDF Library Manager dialog box. The basic setup of the continuous fiber model is performed automat-

ically when the fiber module is successfully loaded.

Opening library "/.../addons/fiber"...

Library "/...addons/fiber/lnx86/3d/libudf.so" opened

fm_adjust

fm_src_mass

fm_src_x_mom

fm_src_y_mom

fm_src_z_mom

fm_src_enthalpy

fm_src_dom

fm_on_demand Done.

Addon Module: fiber...loaded!

If you did not preset the fiber model specific UDF hooks, you will need to check allocation of user-

defined memory, hook an adjust function (fm_adjust) to ANSYS Fluent, and set up the source terms

on your own. This is explained is User-Defined Memory and the Adjust Function Setup (p. ).

Important

Note that user-defined memory locations for the fiber model will not be allocated properly

if you do not initialize the flow field. If you are setting up a fiber computation based on a

converged case, you must re-load the ANSYS Fluent data file after initializing the solution.

The continuous fiber module setup is saved with the ANSYS Fluent case file. The module is loaded

file, the continuous fiber module is saved with the absolute path. Therefore, if the locations of the

continuous fiber module installation or the saved case file are changed, then ANSYS Fluent will not be

able to load the module when the case file is subsequently read. In this situation, you will have to unload

the UDF library using the UDF Library Manager dialog box after the case file is read, and then reload

the continuous fiber module. To unload the UDF library go to the UDF Library Manager dialog box

User Defined → User Defined → Functions → Manage...

select the fiber library under UDF Libraries, and click Unload. Previously-saved continuous fiber model

setup and parameters will be preserved in this process.

The continuous fiber model is implemented by user-defined functions (UDFs) and scheme routines in

ANSYS Fluent. A number of UDFs are used to solve the fiber equations. When you loaded the fiber

module in the previous step (Loading the Continuous Fiber Module (p. )), UDF and scheme libraries

that are required by the continuous fiber model were automatically loaded. Before you can begin the

process of defining your fiber model, however, you will need to perform some additional setup tasks

that involve allocating user-defined memory for the UDFs and hooking an adjust UDF to ANSYS Fluent.

Follow the procedure below.

Getting Started With the Continuous Fiber Module

... User-Defined Memory and the Adjust Function Setup

... Source Term UDF Setup

. Allocate user-defined memory for the model by incrementing the Number of User-Defined Memory

Location to  in the User-Defined Memory dialog box.

User Defined → User Defined → Memory...

Important

Note that you must initialize your solution (in the Solution Initialization task page) in

order for user-defined memory to be allocated properly. If you are setting up a fiber

simulation based on a converged case, then you will have to reload the ANSYS Fluent

data file after initializing the solution.

. Hook the adjust function UDF to ANSYS Fluent by choosing fm_adjust::fiber from the drop-down

list for Adjust in the User-Defined Function Hooks dialog box.

User Defined → User Defined → Function Hooks...

If you answered no to presetting all fiber model-specific UDF hooks during the loading process

(Loading the Continuous Fiber Module (p. )) then you will need to set source terms, individually,

for each fluid zone in your model. Alternatively, you can leave the default settings (none for no source

term).

For each fluid zone in your model, specify none, constant, or UDF for all of the source terms by

following the procedure below:

Setup →

. In the Cell Zone Conditions task page, select a fluid zone under Zone and click edit....This opens the

Fluid dialog box.

. In the Fluid dialog box, check Source Terms and click the Source Terms tab.

. For each of the source terms in the scroll list (Mass, X Momentum, and so on), click the Edit... button

next to each source term to open the corresponding source dialog box. Leave the default none, or choose

constant or UDF from the drop-down list. Choose the UDF in the drop-down list that corresponds to

the particular source term. For example, udf fm_src_mass corresponds to the Mass source term. Use

the table below (Table . : Source Terms and Corresponding UDFs (p. )) as a reference guide.

Table . : Source Terms and Corresponding UDFs

udf fm_src_mass

Mass

udf fm_src_x_mom

X Momentum or Axial Momentum

udf fm_src_y_mom

Y Momentum or Radial Momentum

udf fm_src_z_mom

Z Momentum

udf fm_src_enthalpy

Energy

udf fm_src_dom

discrete ordinates model

. Click OK when all of the UDFs have been hooked.

. Repeat this process for the remaining fluid zones in your ANSYS Fluent model.

Important

If you want to include radiative interaction of the fibers with the discrete ordinate (DO)

radiation model, then the appropriate source term UDF (udf fm_src_dom) will be

hooked automatically when you select Fiber Radiation Interaction in the Fiber Model

dialog box. You must initialize the solution (which will allocate memory for the DO

model) before the fiber model will be ready to accept the fiber radiation interaction

data.

This section provides information on how to choose the type of fiber model you want to implement

as well as select various model options that are available in ANSYS Fluent’s fiber model. The fiber

Model and Options are selected in the Fiber Model dialog box (Figure . : The Fiber Model Dialog

Box (p. )).

Setup → Models → Continuous Fiber Spinning

Edit...

Fiber Models and Options

Figure . : The Fiber Model Dialog Box

... Choosing a Fiber Model

... Including Interaction With Surrounding Flow

... Including Lateral Drag on Surrounding Flow

... Including Fiber Radiation Interaction

...Viscous Heating of Fibers

... Drag, Heat and Mass Transfer Correlations

With ANSYS Fluent’s fiber model, you can model two types of fibers: melt spun and dry spun. The

model you choose depends on the polymer that is used to draw the fibers. If the fiber polymer can

be molten without being destroyed thermally, then a melt spun fiber process is typically used to produce

the fibers. In such cases, select Melt Spun Fibers under Model in the Fiber Model dialog box (Fig-

ure . : The Fiber Model Dialog Box (p. )).

When the fiber polymer can be liquefied with a suitable solvent, or the fiber polymer’s production

process involves a solvent, the fibers are formed typically in a dry spinning process. In such cases, select

Dry Spun Fibers under Model in the Fiber Model dialog box (Figure . : The Fiber Model Dialog

Box (p. )).

If the fibers in your simulation strongly influence the flow of the surrounding fluid and need to be

considered, you must select Interaction with Fluent under Options in the Fiber Model dialog box

(Figure . : The Fiber Model Dialog Box (p. )). When iterating a solution with ANSYS Fluent, the

fiber model equations are solved alternating with ANSYS Fluent’s flow equations. Source terms are

also computed to couple the fiber equations with the fluid flow equations. The calculation of the

source terms is performed only during the course of an ANSYS Fluent computation. See Coupling

Between Fibers and the Surrounding Fluid for a description of the source terms.

In typical fiber simulations, the axial drag of the fibers is the most important force acting on the fibers

as well as on the surrounding fluid. In some situations, the lateral or cross-flow drag can become im-

portant. This is the case when the fibers are mainly cooled or dried in a cross-flow situation. In such

cases you can select Include Lateral Drag under Options in the Fiber Model dialog box (Fig-

ure . : The Fiber Model Dialog Box (p. )). The drag is estimated for a cylinder in cross-flow and is

shown in Equation .. Lateral drag is not considered by the fiber equations and therefore lateral

bending of the fibers is not considered.

In some situations radiative heat exchange is important. If you are using ANSYS Fluent’s P- radiation

model or ANSYS Fluent’s discrete ordinates (DO) radiation model, you can consider the effects of irra-

diation on the cooling and heating of the fibers. When you are using the DO radiation model, the effects

of the fibers upon the DO model can be considered. If the DO radiation model is enabled, you can

select Fiber Radiation Interaction (Options group box) and enter the fiber’s Emissivity in the Prop-

erties group box (see Figure . : The Fiber Model Dialog Box (p. )).

When high elongational drawing rates are combined with large fiber viscosities, viscous heating of

fibers may become important. To consider this effect in the fiber energy equation (Equation . ),

you can select Fiber Viscous Heating under Options in the Fiber Model dialog box (Figure . : The

Fiber Model Dialog Box (p. )).

The effects of the boundary layer of the fiber are modeled in terms of drag, heat transfer, and mass

transfer coefficients. These parameters are specified under Exchange in the Fiber Model dialog box

(Figure . : The Fiber Model Dialog Box (p. )).

For the Drag Coefficient, you can choose between const-drag, kase-matsuo, gampert and user-defined

from the drop-down list. If you choose const-drag, the constant you enter must be specified as a dimen-

sionless value. See Drag Coefficient for a description of these options. User-defined functions (UDFs) are

described in detail in User-Defined Functions (UDFs) for the Continuous Fiber Model (p. ).

For the Heat Transfer Coefficient you can choose between const-htc, kase-matsuo-, kase-matsuo-,

gampert, and user-defined from the drop-down list. If you choose const-htc, the constant you enter must

be specified SI units of

. See Heat Transfer Coefficient for a description of these options. User-

defined functions (UDFs) are described in detail in User-Defined Functions (UDFs) for the Continuous Fiber

For the Mass Transfer Coefficient you can choose between const-mtc, kase-matsuo-, kase-matsuo-,

gampert, and user-defined. If you choose const-mtc, you must enter the mass transfer rate in units of

instead of the mass transfer coefficient. See Mass Transfer Coefficient for a description of these

options. User-defined functions (UDFs) are described in detail in User-Defined Functions (UDFs) for the

Continuous Fiber Model (p. ).

...The Concept of Fiber Materials

... Description of Fiber Properties

The material properties you specify for the fibers are used for all fibers defined in your model. You

cannot consider fibers consisting of different fiber materials in one simulation.

The continuous fiber model makes use of ANSYS Fluent’s material concept for the Material Type of

the fluid. Because not all properties are available in ANSYS Fluent’s Create/Edit Materials dialog box

for this material type, some additional property information can be provided through the Fiber Model

dialog box (Figure . : The Fiber Model Dialog Box (p. )). The procedure to define the material

properties for the fibers in your simulation is as follows:

. In the Create/Edit Materials dialog box, set the Material Type as fluid.This fluid will be used as the

polymer or solvent in the fiber.

. Enter all data for this material.

You can use all profiles available in the Create/Edit Materials dialog box to define the properties

as functions of temperature. In order to invoke user-defined fiber properties, you need to use the

UDF template file (see User-Defined Functions (UDFs) for the Continuous Fiber Model (p. ) for

details). UDF access is available for viscosity, density, specific heat capacity, thermal conductivity

and solvent liquid-vapor equilibrium pressure.

. Select the Polymer in the Materials group box of the Fiber Model dialog box.

. For dry spinning simulations, you also have to select Solvent and the gas phase species that represents

the Solvent Vapor.

. Enter any additional data needed for the fiber material in the Fiber Model dialog box.

The properties that appear in the Fiber Model dialog box vary depending on the fiber model type.

The following list describes the properties you may need for a fiber material. For every property listed,

the dialog box name is provided where the property can be defined.

Blending Interval

(Fiber Model dialog box) is the temperature interval used to compute an average of the fiber viscosities

in liquid and solid state of Melt Spun Fibers.This option is only available when the Melt Spun Fibers

option is selected. See Fiber Viscosity for details about how the Blending Interval is applied to the fiber

viscosity.

Cp

(Create/Edit Materials dialog box) is the specific heat,

, of the fiber in units of energy per mass and

temperature. In the case of dry spun fibers, a mass average is computed based on the values entered for

Polymer and its Solvent.You can use any of the functions available to define temperature dependency.

If you want to use a user-defined function profile, you need to modify the UDF template provided by

ANSYS Fluent. See User-Defined Functions (UDFs) for the Continuous Fiber Model (p. ) for details.

Density

(Create/Edit Materials dialog box) is the density,

, of the fiber in units of mass per unit volume.This

density is the mass density and not the volume density. In the case of dry spun fibers, a mass average is

computed based on the values entered for Polymer and its Solvent.You can use any of the functions

available to define temperature dependency. If you want to use a user-defined function profile, you need

to modify the UDF template provided by ANSYS Fluent. See User-Defined Functions (UDFs) for the Con-

tinuous Fiber Model (p. ) for details.

Emissivity

(Fiber Model dialog box) is the emissivity of fibers in your model,

, used to compute radiation heat

transfer to the fibers (Equation ., Equation ., Equation . and Equation .) when the P-

or discrete ordinates radiation model is active. Note that you must enable radiation to fiber, using the

Fiber Radiation Interaction option in the Fiber Model dialog box.

Flory Huggins

(Fiber Model dialog box) can be enabled to apply Equation . to compute the vapor-liquid equilibrium

at the fiber surface.When it is enabled, you have to specify an appropriate value for the dimensionless

Flory Huggins parameter,

.This option is only visible when Dry Spun Fibers has been chosen.

(Fiber Model dialog box) is the latent heat of vaporization of the Solvent when evaporated from a dry

spun fiber. Note that you have to enter the vaporization or reference temperature,

, where the specified

value of the latent heat has been measured.This vaporization temperature is used to automatically consider

the change of latent heat with temperature. See Equation . and Equation . for more information

on how this is achieved.These options are only visible when Dry Spun Fibers has been chosen.

Solidification Temperature

(Fiber Model dialog box) is the temperature below which the fiber polymer of a Melt Spun Fiber will

solidify. It will be used when computing the viscosity of Melt Spun Fibers.This option is only visible

when Melt Spun Fibers has been chosen.

Solvent Vapor Pressure

(Fiber Model dialog box) is the vapor pressure of the solvent evaporating from the fiber surface in dry

spinning.You have to enter coefficients for an Antoine-type equation (Equation . ). Note that the

coefficients must be entered in such units that the outcome of the Antoine-type equation is in Pascal. In

addition to the coefficients of the Antoine equation, you have to enter the range of validity for the vapor

pressure. Below the minimal temperature the vapor pressure at the minimal temperature will be used.

Above the maximal temperature, the vapor pressure at the maximal temperature is used.

Fiber Material Properties

(Create/Edit Materials dialog box) is the thermal conductivity,

, of the fiber in units of power per length

and temperature. In the case of dry spun fibers, a mass average is computed based on the values entered

for Polymer and its Solvent.You can use any of the functions available to define temperature dependency.

Zero Shear Viscosity

(Create/Edit Materials dialog box and/or the Fiber Model dialog box, depending on the chosen fiber

model) is the fiber viscosity,

, at zero shear rate. It is not the elongational or Trouton viscosity.

For Melt Spun Fibers, you have to enter the viscosity of the fiber in solid state in the Create/Edit

Materials dialog box for the fluid you have selected as the fiber polymer. Typically this value will

be very high compared to the liquid fiber viscosity to represent the fibers as solids. For the solid

fiber viscosity you can make use of any temperature-dependent function available in the Create/Edit

Materials dialog box. If you want to use a user-defined function profile, you need to modify the

UDF template provided by ANSYS Fluent. See User-Defined Functions (UDFs) for the Continuous

Fiber Model (p. ) for details.

In the Fiber Model dialog box, you have to enter the coefficients for the fiber viscosity in liquid

state (Equation . ). To define viscosity as a function of fiber velocity gradient, set

to a value

different than . In the case of Melt Spun Fibers, you also have to enter data for the Solidification

Temperature and the Blending Interval. The blending of the viscosities in liquid and solid state

will be computed based on Equation ..

For Dry Spun Fibers you only have to enter the coefficients for Equation . in the Fiber Model

dialog box. To specify fiber viscosity as a function of fiber velocity gradient, set

to a value different

than . Any value entered in the Create/Edit Materials dialog box for viscosities of the fluids used

as fiber polymer and fiber solvent will not be considered.

Note

Note that depending on fiber velocity gradient, the numerical behavior of the Fiber

Model equations may become unstable in combination with fiber viscosity.

... Fiber Injection Types

...Working with Fiber Injections

... Defining Fiber Injection Properties

... Point Properties Specific to Single Fiber Injections

... Point Properties Specific to Line Fiber Injections

... Point Properties Specific to Matrix Fiber Injections

... Define Fiber Grids

The primary inputs that you must provide for the continuous fiber model calculations in ANSYS Fluent

are the starting positions, mass flow rate, take up positions, and other parameters for each fiber. These

provide the boundary conditions for all dependent variables to be solved in the continuous fiber

model. The primary inputs are:

Start point ( ,

,  coordinates) of the fiber.

Number of fibers in group. Each defined fiber can represent a group of fibers that will be used only to

compute the appropriate source terms of a group of fibers.

Diameter of the fiber nozzle,

.

Mass flow rate per nozzle to compute the velocity of the fiber fluid in the nozzle.The velocity is used as

.

boundary condition for the fiber momentum equation.

Temperature of the fiber at the nozzle,

.

Solvent mass fraction of the fiber fluid in the nozzle.This value is used as boundary condition for the solvent

continuity equation.

Take-up point ( ,

Velocity or force at take-up point to describe the second boundary condition needed for the fiber momentum

equation (see Equation . ).

In addition to these parameters, you have to define parameters for the grid that is distributed between

the start position and take-up point of the fibers. On this grid the dependent fiber variables are solved,

by discretizing Equation ., Equation ., and Equation ..

You can define any number of different sets of fibers provided that your computer has sufficient

memory.

You will define boundary conditions and grids for a fiber by creating a fiber “injection” and assigning

parameters to it. In the continuous fiber model the following types of injections are provided:

single

Use this option to define a single fiber.

line

Use this option when the fibers you want to define start from a line and the starting points are

located at constant intervals on this line.

matrix (only in 3D)

Use this option when the fiber starting points are arranged in the shape of a rectangle.

file

Use an ASCII file for entering coordinates and material properties of individual fiber injections in a

tabular format as shown below.

;  1st commentary line

;  2nd commentary line

;  m-th commentary line

Defining Fibers

x1   y1   z1   df1   m1   Tf1   Ys1

x2   y2   z2   df2   m2   Tf2   Ys2

... ...  ...  ...  ...  ...  ...

xn   yn   zn   dfn   mn   Tfn   Ysn

where each injection is described by the following data fields, all on one line, separated by spaces:

x, y, and z are the Cartesian coordinates of the injection point. The z coordinate must be

included for both 3D and 2D solvers to maintain the sequence in which the data entries are

interpreted, however, the z coordinate is not used in 2D.

df is the fiber diameter

m is the mass flow rate

Tf is the temperature

Ys is the solvent liquid mass fraction (ignored for melt spinning)

You can include an arbitrary number of comments anywhere in the file. Commentary lines must

begin with a semicolon (;).

Figure . : The Fiber Injections Dialog Box

You will use the Fiber Injections dialog box (Figure . : The Fiber Injections Dialog Box (p. )) to

create, modify, copy, delete, initialize, compute, print, read, write, and list fiber injections. To access

the Fiber Injections dialog box, first make sure you enable a fiber model, then go to

Setup → Models → Fiber-Injections

Edit...

.... Creating Fiber Injections

To create a fiber injection, click Create. A new fiber injection appears in the Fiber Injections list and

the Set Fiber Injection Properties dialog box opens automatically to enable you to specify the fiber

injection properties (as described in Point Properties Specific to Single Fiber Injections (p. )).

.... Modifying Fiber Injections

To modify an existing fiber injection, select its name in the Fiber Injections list and click Set.... The

Set Fiber Injection Properties dialog box opens, and you can modify the properties as needed.

.... Copying Fiber Injections

To copy an existing fiber injection to a new fiber injection, select the existing injection in the Fiber

Injections list and click Copy. The Set Fiber Injection Properties dialog box will open with a new

fiber injection that has the same properties as the fiber injection you have selected. This is useful if

you want to set another injection with similar properties.

.... Deleting Fiber Injections

You can delete a fiber injection by selecting its name in the Fiber Injections list and clicking Delete.

.... Initializing Fiber Injections

To initialize all solution variables of the fibers defined in a fiber injection, select its name in the Fiber

Injections list and click Initialize. The solution variables will be set to the boundary condition values

at the starting points of the fibers.

You can select several fiber injections when you want to initialize several fiber injections at one time.

Important

If you do not select a fiber injection and click Initialize, all fiber injections will be initialized.

.... Computing Fiber Injections

To solve the fiber equations of a fiber injection for a number of iterations, select its name in the Fiber

Injections list and click Compute. The solution variables of the fibers defined in this fiber injection

will be updated for the number of iterations specified in Figure . : Fiber Solution Controls Dialog

Box (p. ).

Box (p. ).

You can select several fiber injections when you want to compute several fiber injections at one time.

Important

If you do not select a fiber injection and click Compute, all fiber injections will be computed.

.... Print Fiber Injections

To print the fiber solution variables of a fiber injection into a file, select its name in the Fiber Injections

list and click Print. A file name is generated automatically based on the name of the fiber injection

and the number of the fiber. The solution variables of each fiber is stored in a separate file. You may

use this file for an external postprocessing or analysis of fiber data.

You can select several fiber injections when you want to print several fiber injections at one time.

Important

If you do not select a fiber injection and click Print, all fiber injections will be printed.

.... Read Data of Fiber Injections

To read the data (properties and solution variables) of a fiber injection previously stored in a file, click

Read Data. A file selection dialog box is opened where you can select the name of the file in a list

or you can enter the file name directly. The names of all fiber injections included in the file are com-

pared with the fiber injections already defined in the model. If the fiber injection exists already in

your model, you are asked to overwrite it.

....Write Data of Fiber Injections

While the settings of the continuous fiber model for numerics and models are stored in the ANSYS

Fluent case file, the data of the fibers and defined injections have to be stored in a separate file. To

write the data of a fiber injection to a file, click Write Data. A file selection dialog box is opened

where you can select the name of an existing file to overwrite it or you can enter the name of a new

file.

You can select several fiber injections when you want to store several fiber injections in one file.

Important

If you do not select a fiber injection and click Write Data, all fiber injections will be stored

in the specified file.

....Write Binary Data of Fiber Injections

To write the data of a fiber injection in binary format to a file, click Write Binary Data. A file selector

dialog box is opened where you can select the name of an existing file to overwrite it or you can

enter the name of a new file.

You can select several fiber injections when you want to store several fiber injections in binary format

in one file.

Important

If you do not select a fiber injection and click Write Binary Data, all fiber injections will

be stored in binary format in the specified file.

.... List Fiber Injections

To list starting positions and boundary conditions of the fibers defined in a fiber injection, click List.

ANSYS Fluent displays a list in the console window. For each fiber you have defined, the list contains

the following (in SI units):

File number in the injection in the column headed (NO).

,

, and  position of the starting point in the columns headed (X), (Y), and (Z).

Fiber velocity in the column headed (U).

Temperature in the column headed (T).

Solvent mass fraction in the column headed (SOLVENT).

Diameter in the column headed (DIAM).

Mass flow rate in the column headed (MFLOW).

The number of fibers represented by this fiber group in the column headed (FIBERS).

The number of fiber grid cells defined for this fiber in the column headed (CELLS).

A notification whether the starting point of the fiber is located inside or outside the domain in the column

headed (IN DOMAIN? ).

The boundary conditions at the take up point are also listed. This list consists of the following (in SI

units):

,

, and  position of the take-up point in the columns headed (X), (Y), and (Z).

Boundary condition type and its specified value (VELOCITY for given take-up velocity, FORCE for given

force in the fiber) in the column headed (BOUNDARY CONDITION).

You can select several fiber injections when you want to list several fiber injections.

Important

If you do not select a fiber injection and click List, all fiber injections will be listed.

Once you have created an injection (using the Fiber Injections dialog box, as described in Creating

Fiber Injections (p. )), you will use the Set Fiber Injection Properties dialog box (Figure . : The

Set Fiber Injection Properties Dialog Box (p. )) to define the fiber injection properties. (Remember

that this dialog box opens when you create a new fiber injection, or when you select an existing fiber

injection and click Set... in the Fiber Injections dialog box.)

Figure . : The Set Fiber Injection Properties Dialog Box

The procedure for defining a fiber injection is as follows:

.

.

If you want to change the name of the fiber injection from its default name, enter a new one in the Fiber

Injection Name field.This is recommended if you are defining a large number of injections so you can

easily distinguish them.

.

Choose the type of fiber injection in the Fiber Injection Type drop-down list.The three choices (single,

line, and matrix) are described in Fiber Injection Types (p. ).

.

Click the Injection Point Properties tab (the default), and specify the point coordinates according to

the fiber injection type, as described in Point Properties Specific to Single Fiber Injections (p. )–Point

Properties Specific to Matrix Fiber Injections (p. ).

.

If each of the defined fibers is referring to a group of fibers, enter the number of fibers in Number of

Fibers in Group. If your nozzle plate has  holes and you can simulate them as a line fiber injection

with  groups, you have to enter a value of .This means that only  fibers are solved numerically, but

each of these fibers stands for  fibers to be used to compute the source terms for the surrounding

fluid.This enables you to reduce computing efforts while achieving a proper coupling with the surrounding

fluid.

Important

Note that the Number of Fibers in Group is applied to all fibers, defined in your injec-

tion. If the number of fiber groups in your line or matrix injection is not the same for

all fibers in this injection, you should split this injection into several fiber injections.

.

Specify the diameter of the nozzle in the Diameter field.

.

.

.

Enter the mass flow rate for a single nozzle in the Flow rate per Nozzle field.This will be used to compute

the starting velocity of the fiber fluid.

Important

Note that the value specified refers to one single nozzle and not to the mass flow rate

of all fibers defined in this fiber injection.

.

Specify the temperature of the fiber fluid leaving the nozzle in the Temperature field.

.

If you are modeling dry spun fibers you also have to enter the solvent’s mass fraction at the nozzle in

the Solvent Mass Fraction field.

Figure . : The Set Fiber Injection Properties Dialog Box With Take-Up Point Properties

.

Click the Takeup Point Properties tab and enter the coordinates of the take-up point (see Figure . :The

Set Fiber Injection Properties Dialog Box With Take-Up Point Properties (p. )).

Important

Note that all fibers defined in the fiber injection are collected at the same point. If the

fibers of your line or matrix injection vary in this property, you have to define them

using several fiber injections.

. Select the appropriate boundary condition from the Boundary Condition drop-down list and specify

the value for this boundary condition. Choose prescribed-velocity if you know the drawing or take-up

velocity. Choose tensile-force if you want to prescribe a given tensile force in the fiber at the take-up

point.

. Click the Grid Properties tab and enter all data needed to generate the fiber grid as described in Define

Fiber Grids (p. ).

For a single fiber injection, you have to specify the coordinates of the starting point of the fiber. Click

the Injection Point Properties tab and set the ,

, and  coordinates in the x0, y0, and z0 fields of

the Points box. (z0 will appear only for 3D problems.)

In a line fiber injection the starting points of the fibers are arranged on a line at a constant distance

(see Figure . : Line Injections (p. )). You have to specify the coordinates of the starting point and

the end point of this line. Click the Injection Point Properties tab in the Set Fiber Injection Properties

dialog box (Figure . : The Set Fiber Injection Properties Dialog Box (p. )). In the Points region, set

the ,

, and  coordinates in the x0, y0, and z0 fields for the starting point of the line and the ,

,

and  coordinates in the x1, y1, and z1 fields for the end point of the line. (z0 and z1 will appear only

for 3D problems.)

Figure . : Line Injections

In addition to the coordinates, you have to set the number of fibers defined in the line injection by

entering the appropriate value in the Point Density Edge1 field. See Figure . : Line Injections (p. )

for an example of a line fiber injection with a Point Density Edge1 of .

In a matrix fiber injection the starting points of the fibers are arranged in several rows having the

shape of a rectangle or a parallelogram. Each row has the same distance to the previous and is divided

into equal sections (see Figure . : Matrix Injections (p. )).

You have to specify the coordinates of the starting point and the end of point of the first row and the

coordinates where the last row should start. Click the Injection Point Properties tab in the Set Fiber

Injection Properties dialog box (Figure . : The Set Fiber Injection Properties Dialog Box (p. )). In

the Points region, set the ,

, and  coordinates in the x0, y0, and z0 fields for the starting point

and the ,

, and  coordinates in the x1, y1, and z1 fields for the end point of the first row of fibers.

The ,

, and  coordinates of the starting point of the last row have to be entered in the x2, y2, and

z2 fields.

At each row, the number of fibers specified in the Point Density Edge1 field are injected. The number

of rows to be injected is specified in Edge2.

You can double check the number of fibers computed in this fiber injection if you inspect the Numbers

of Fibers Computed field.

Important

Note that this fiber injection type is only available for 3D problems.

Figure . : Matrix Injections

Each fiber consists of a straight line between the injection point and the take-up point. It is divided

into a number of finite volume cells. Every fiber defined in a fiber injection has its own grid, which

you can specify if you click the Grid Properties tab in the Set Fiber Injection Properties dialog box.

.... Equidistant Fiber Grids

To define an equidistant grid for the fibers select equidistant from the Grid Type drop-down list.

Specify the Number of Cells into which every fiber of the fiber injection will be divided.

Figure . : Equidistant Fiber Grid

.... One-Sided Fiber Grids

A one-sided grid is graded near the injection point of the fiber. To define a one-sided grid for the

fibers select one-sided from the Grid Type drop-down list. Specify the Number of Cells into which

every fiber of the fiber injection will be divided. In addition, you have to specify the ratio,

, between

each subsequent fiber cell in the Grid Growth Factor at Injection Point field. Values larger than

refine the grid, while values smaller than  coarsen the grid.

Figure . : One-Sided Fiber Grid

....Two-Sided Fiber Grids

A two-sided grid is graded near the injection point as well as at the take-up point of the fiber. To

define a two-sided grid for the fibers, select two-sided from the Grid Type drop-down list. Specify

the Number of Cells into which every fiber of the fiber injection will be divided. You also have to

specify the ratio,

, between each subsequent fiber cell at the injection point in the Grid Growth

Factor at Injection Point field and the ratio,

, near the take-up point in the Grid Growth Factor

at Takeup Point field. Values larger than  refine the grid, while values smaller than  will coarsen

it.

Figure . : Two-Sided Fiber Grid

....Three-Sided Fiber Grids

A three-sided grid consists of three sides where the fiber grid can be graded. The first side is near

the injection point. The other two sides are around a refinement point within the fiber grid. Both

sides at the refinement point are graded at the same ratio between the fiber grid cell lengths. To

define a three-sided grid for the fibers, select three-sided from the Grid Type drop-down list (see

Figure . : Defining a Three-Sided Fiber Grid Using the Set Fiber Injection Properties Dialog

Box (p. )). Specify the Number of Cells until Grid Refinement Point, the Grid Growth Factor at

Injection Point, and the Grid Growth Factor at Local Grid Refinement Point. You also have to

specify the location of the grid refinement point in the Location of Local Grid Refinement Point

field in a dimensionless way. The value you have to enter is relative to the fiber length and may be

between  and . Values larger than  refine the grid, while values smaller than  coarsen the grid.

Click the Compute button to estimate the Number of Cells behind Grid Refinement Point.

Figure . : Three-Sided Fiber Grid

Box

The continuous fiber model enables you to apply custom correlations for drag, heat transfer, mass

transfer coefficients, as well as material properties to the fibers by means of user-defined functions

(UDFs). You are provided with a C template file named fiber_fluent_interface.c that contains

source code for the drag, heat transfer, mass transfer coefficient, and the fiber property UDFs. You will

need to modify this UDF source file to suit your application, compile it, and hook the resulting UDF

object(s) to the fiber model. This process is described below.

... UDF Setup

... Customizing the fiber_fluent_interface.c File for Your Fiber Model Application

... Compile Fiber Model UDFs

... Hook UDFs to the Continuous Fiber Model

Before you can edit the UDF template and create your custom UDF for drag, heat transfer or mass

transfer coefficient, you must copy the fiber directory to your working directory. The fiber directory

contains all of the libraries and support files that are required to compile UDFs for the fiber model and

build shared libraries for the architecture that you specify.

Make a local copy of the fiber directory by copying it from the path below to your working directory.

path/ansys_inc/v195/fluent/fluent19../addons/fiber/

where path  is the directory in which you have installed ANSYS Fluent.

.

Open a Visual Studio .NET DOS prompt.

.

Make a local copy of the fiber folder (not a symbolic link) by copying it from the folder below to your

working folder.

path\ANSYS Inc\v195\fluent\fluent19..\addons\fiber\

where path  is the folder in which you have installed ANSYS Fluent (by default, the path is

C:\Program Files).

... Customizing the fiber_fluent_interface.c File for Your Fiber Model

Application

Now that you have copied the fiber directory to your working directory, you can edit the UDF

template file and customize it to fit your model needs.

.

In your working directory, change directories to fiber/src.The /src directory contains the UDF

template source file fiber_fluent_interface.c.

.

.

.

In the /src directory, use any text editor and edit fiber_fluent_interface.c.

.

Scroll down to the bottom of the fiber_fluent_interface.c file to the section that contains

concatenated functions for friction factor (drag coefficient), heat transfer coefficient, mass transfer

coefficient, fiber viscosity, fiber density, fiber thermal conductivity, fiber specific heat, and vapor liquid

equilibrium, respectively.These are the UDFs that you can modify and customize.

User-Defined Functions (UDFs) for the Continuous Fiber Model

.

Edit the function(s) you require for your particular application. Save fiber_fluent_interface.c

and overwrite the existing file.

Important

Do not save the file with another name because it will not be recognized by the system.

Important

The function names of the templates user_friction_factor,

user_heat_transfer_coefficient, and user_mass_transfer_coeffi-

cient must not be altered because they are called by other routines in the continuous

fiber model.

.... Example: Heat Transfer Coefficient UDF

Below is an example of a heat transfer coefficient UDF that is defined in fiber_fluent_inter-

face.c. The function is taken from Kase and Matsuo  and is implemented as the kase-matsuo-

option in the fiber model. The function name user_heat_transfer_coefficient must not,

under any circumstances, be altered because it is called by other functions in the continuous fiber

model.

There are two arguments to the user_heat_transfer_coefficient UDF: Fiber and Loc-

al_Fiber_Data_Type. Fiber *f is a pointer to the fiber structure that contains information

model.

about the fiber and Local_Fiber_Data_Type *fd accesses temporary variables that are needed

during the calculation of the fiber.

In the sample UDF below, a loop is performed over all fiber grid cells using the macro FIB_N(f)

which represents the number of grid cells for the fiber f. The Reynolds number is computed based

on the relative velocity,

(ABS(FIB_C_U(f,i)-fd->up[i])); the fiber diameter,

FIB_C_D(f,i); the density of the surrounding fluid, fd->rho[i] and the viscosity of the surround-

ing fluid, fd->vis[i]. The heat transfer coefficient  is computed from the Nusselt number using

the thermal conductivity of the surrounding fluid,

, (fd->k[i]) and is stored in fd->alpha[i].

void

user_heat_transfer_coefficient(Fiber *f, Local_Fiber_Data_Type *fd)

{

int i;

real Red, Nud;

/* model from Kase/Matsuo () */

for (i=; iFIB_N(f); i++)

{

/* compute Reynolds number based on relative velocity */

Red = ABS(FIB_C_U(f,i)-fd->up[i])*FIB_C_D(f,i)*fd->rho[i]/fd->vis[i];

Nud = . *pow(Red, . );

/* store heat transfer coefficient for latter use */

fd->alpha[i] = Nud*fd->k[i]/FIB_C_D(f,i);

}

}

All variables and macros that are used in user_heat_transfer_coefficient are defined in

header files provided with the continuous fiber model. For example, you will find the type definition

Fiber and the macros that are used to access variables of a single fiber in the header file fiber.h.

Temporary variables used in the type definition of Local_Fiber_Data_Type can be found in the

header file fib-mem.h.

Important

Important

Note that you must not modify the header files provided with the continuous fiber model.

Otherwise the compiled library will not be compatible with ANSYS Fluent and will show

run time errors.

.... Example: Fiber Specific Heat Capacity UDF

You can also calculate fiber material properties using UDFs. ANSYS Fluent provides a UDF template

for every fiber property. You can modify the UDF templates for your specific case.

The template for the fiber density is as follows:

real User_Fiber_Specific_Heat(Fiber *f, real temp, real liq, int i)

{

real yi[MAX_SPE_EQNS];

real cp_p;

/* compute cp based on FLUENT's standard procedure selected in materials panel */

cp_p = Specific_Heat(FIB_MATERIAL_POLYMER(f), temp, ., yi);

if (FIB_DRY_SPINNING(f))

{

real cp_s;

cp_s = Specific_Heat(FIB_MATERIAL_SOLVENT(f), temp, ., yi);

return cp_p*(.-liq)+cp_s*liq;

}

return cp_p;

}

Important

The function names of the templates User_Friction_Factor, User_Heat_Trans-

fer_Coefficient, User_Mass_Transfer_Coefficient, User_Fiber_Viscos-

ity, User_Fiber_Density, User_Fiber_Thermal_Conductivity,

User_Fiber_Specific_Heat, and User_Fiber_Vle must not be altered since they

are called by other routines of the continuous fiber model.

All variables and macros defined in the header files are provided with the continuous fiber model.

For example, you will find the type definition Fiber and the macros to access variables of a single

fiber in the header file fiber.h. The temporary variables used in the type definition of Loc-

al_Fiber_Data_Type can be found in the header file fib-mem.h.

Important

Important

You must not modify the header files provided with the continuous fiber model. Otherwise

the compiled library will not be compatible with ANSYS Fluent resulting in runtime errors

(messages will be printed in the console).

Once you have customized the UDF template fiber_fluent_interface.c for your fiber model

application, you are now ready to compile the source file using the text interface. Follow the procedure

below for Linux Systems and Windows Systems, respectively.

In the /fiber in your working directory, run the make command that will compile your fiber mode

UDF and build a shared library for the architecture you are running. To do this, type the following

command at the prompt:

make -f Makefile-client FLUENT_ARCH=your_arch

where your_arch is replaced by the architecture of the machine you are running (for example,

lnx86).

For example, if your computer architecture is lnx86 type the following command in a terminal session:

make -f Makefile-client FLUENT_ARCH=lnx86

To identify the architecture of the machine you are running on, scroll up the ANSYS Fluent console

window to the message that begins with “Starting”.

When you run the make process, the source code (fluent_fiber_interface.c) will be compiled

into object code and a shared library will be built for the computer architecture and version of ANSYS

Fluent you are running. Messages about the compile/build process will be displayed on the console

window. You can view the compilation history in the log file that is saved in your working directory.

Below is an example of console messages for a lnx86 architecture running a 2D version of ANSYS

Fluent.

Working...

for d in lnx86[]*; do \

( \

cd $d; \

for f in ../../src*. [ch] ../../src/makefile; do \

if [ ! -f ’basename $f’ ]; then \

echo "# linking to " $f "in" $d; \

ln -s $f . ; \

fi; \

done; \

echo ""; \

echo "# building library in" $d; \

make -kmakelog &; \

cat makelog; \

) \

done

# linking to ...  myudf.c in lnx86/2d

# building library in lnx86/2d

make[]: Entering directory ..../udf_names.c

# Generating udf_names

make[]: Entering directory ..../fluent_fiber_interface.c

make libudf.so ...

# Compiling udf_names.o ...

# Compiling profile.o ...

# Linking libudf.so ...

make[]: Leaving directory ..../udf_names.c

make[]: Leaving directory ..../fluent_fiber_interface.c

You can also see the ’log’-file in

the working directory for compilation history

Done.

.... NT/Windows Systems

. Make a local copy of the fiber folder. Do not create a shortcut.

a.

Create a directory for the custom fiber libraries (for example, /home/custom-build).

b. Copy the fiber library from the installation of ANSYS Fluent (Ansys Inc\v195\fluent\flu-

. Open the Visual Studio .NET DOS prompt (see Compiler Requirements for Windows Systems in the

ANSYS, Inc. Installation Guides for compilers that are compatible with ANSYS Fluent).

. Set the FLUENT_INC environment variable to the current ANSYS Fluent installation directory, for example:

FLUENT_INC="<driveletter>\ANSYS Inc\v195\fluent"

. Enter the fiber\src folder:

cd fiber/src

. Make changes to the fiber_fluent_interface.c file.

. Return to the fiber folder:

cd ..

build_fiber_udf.bat

continuous fiber module in one of following ways:

FLUENT_ADDONS=<driveletter>\home\custom-build

where <driveletter> is the target drive letter including the colon (for example, D:). Note

that there should be no spaces in the above path.

Once you have successfully compiled your continuous fiber model UDF(s), the user-defined option

will appear in drop-down lists for parameters under Exchange in the Fiber Model dialog box (Fig-

ure . : The Fiber Model Dialog Box (p. )). To hook your UDF to a particular fiber model parameter,

simply select user-defined from the drop-down list for Drag Coefficient, Heat Transfer Coefficient,

or Mass Transfer Coefficient and click OK.

If you want to use UDFs to define fiber material properties, select the Enable UDF Properties check

box, and then enable individual property UDFs under the User Defined Properties group box.

To access the Fiber Solution Controls dialog box, go to

Setup → Models → Fiber-Controls

Edit...

Figure . : Fiber Solution Controls Dialog Box

The Fiber Solution Controls dialog box enables you to set common solution parameters for the fiber

equations and their coupling with the surrounding fluid.

Solve

is used to enable and disable the solution of the fiber equations for Momentum (Equation . ), Energy

(Equation . ), and Species (Equation . ).When switching off the solution of one of these equations,

it is not computed for any fibers defined in your model.

Discretization

provides a drop-down list where you can assign to each of the fiber equations one of three different dis-

cretization schemes explained in Discretization of the Fiber Equations.

Underrelaxation

contains all under-relaxation factors for all fiber equations that are being solved in the continuous fiber

model. See Under-Relaxation for additional background information and see Solution Strategies for how

to make use of under-relaxation factors in your solution strategy.

Convergence Criterion

is used to stop the fiber iterations when the residuals of all fiber equations are below the prescribed criteria.

You can define a separate convergence criterion for every fiber equation.

Check Convergence

must be turned on if you want to compare the residuals of the fiber equations with the Convergence

Criterion. If you turn this option off, the given number of fiber iterations will be computed.

Relative Residuals

are used to compute the change of the residual of two subsequent iterations relative to the residual of

the last iteration by applying Equation ..The result of this is compared to the Convergence Criterion

to check whether convergence has been achieved.

Fiber Model Solution Controls

Iterations

defines the number of Fiber Iterations performed every time the fiber equations are updated.

Reporting Interval

sets the number of fiber iterations that will pass before the residuals will be printed.

You can reduce the output to the last fiber iteration by specifying Reporting Interval as . This is

recommended when performing a solution that is coupled with the surrounding flow.

Number of Fluent Iterations per Fiber Computation

sets the number of Fluent iterations before the fiber equations are updated in a solution that is coupled

with the surrounding flow.

Source Term Underrelaxation

factor is used to under-relax the fiber source term exchange to the surrounding fluid. In a converged

solution this value does not influence your predictions.

For additional information on how to set and choose values for the options in the Fiber Solutions

Control dialog box, see Solution Strategies.

After you have completed your inputs and performed any coupled calculations, you can display the

location of the fibers and source terms of the fibers, and you can write fiber data to files for further

analysis of fiber variables.

The following data can be displayed using graphical and alphanumeric reporting facilities:

Graphical display of fiber locations

Exchange terms with surrounding fluid

Fiber solution variables.

... Display of Fiber Locations and Grid Points

... Exchange Terms of Fibers

... Analyzing Fiber Variables

... Running the Fiber Module in Parallel

When you have defined fiber injections, as described in Defining Fibers (p. ), you can display the

location of the fibers using ANSYS Fluent’s Contour plot facility (Figure . : Displaying Fiber Locations

Using the Contours Dialog Box (p. )).

Edit...

Figure . : Displaying Fiber Locations Using the Contours Dialog Box

In the Contours of drop-down list, select Custom Field Functions..., then select fiber-location. The

values in this field are between zero and the number of fiber cells in an ANSYS Fluent grid cell.

You may generate iso-surfaces of constant values of fiber-location to display the fibers in 3D problems.

You can also display the locations of the fibers and their grid discretization using the Fiber Mesh

Display dialog box, which can be accessed from the Results/Graphics/Fiber Mesh tree item.

Postprocessing for the Continuous Fibers

Figure . : The Fiber Mesh Display Dialog Box

The following mesh discretization options are available:

Nodes: displays the end points of fiber volume cells

Edges: displays a line along the path of fibers in the domain

Draw Fluent mesh: Enables the display of the CFD mesh geometry with the mesh display settings specified

in the Mesh Display dialog box.The Mesh Display dialog box will appear automatically when you enable

the Draw Fluent mesh option.

You can set the fiber Line Width in the Fiber Style Attribute dialog box accessed by clicking the

Style Attributes... button.

Figure . : The Fiber Style Attributes Dialog Box

For the injections selected in the Fiber Injections selection list, you can display either all injection

fibers or single fibers with a specified Fiber ID (when the Show Single Fiber option is selected).

The continuous fiber model computes and stores the exchange of momentum, heat, mass, and radiation

in each control volume in your ANSYS Fluent model. You can display these variables graphically by

drawing contours, profiles, and so on. They all are contained in the Custom Field Functions... category

fiber-mass-source

defined by Equation ..

fiber-x-momentum-source

is the x-component of the momentum exchange, defined by Equation ..

fiber-y-momentum-source

is the y-component of the momentum exchange, defined by Equation ..

fiber-z-momentum-source

is the z-component of the momentum exchange, defined by Equation ..

fiber-energy-source

fiber-dom-absorption

fiber-dom-emission

Note that these exchange terms are updated and displayed only when coupled computations are

performed.

You can use ANSYS Fluent’s Plot facilities to analyze fiber solution variables such as fiber velocity,

temperature, diameter, and so on.

.... XY Plots

To investigate fiber variables you have to generate an xy-file for every variable using the following

procedure from the text command interface (assuming that you have already defined a fiber injection):

.

Store an xy-file with the variable of interest.

continuous-fiber → print-xy

.

Enter the fiber injection of interest when asked for

Fiber Injection name>

.

Specify a variable for x-column.This will be used as abscissa in the file plot.

.

Specify another variable for y-column, which will be used as ordinate in the file plot.

.

Specify a file name when asked for XY plot file name.

.

Load the file with ANSYS Fluent’s xy plot facilities, described in the ANSYS Fluent manual.

The following variables can be entered as x-column and y-column:

axial drag

conductivity

curvature

diameter

enthalpy

evaporated mass flux

heat transfer coefficient

lateral drag

length

mass flow

mass fraction

mass transfer coefficient

Nusselt number

Sherwood number

Reynolds number

surface mass fraction

tensile force

user variable

velocity

velocity gradient

viscosity

If a fiber injection consists of several fibers, the data of all fibers in this fiber injection will be stored

in the xy-file.

In addition to this, you can store a fiber history file for a fiber injection as described in Print Fiber In-

jections (p. ). This can be used to analyze a single fiber using ANSYS Fluent xy-plot facilities or by

external postprocessing programs.

.... Fiber Display

To visualize injection fibers, you can use the Fiber Display dialog box, which can be accessed from

the Results/Graphics/Fibers tree item.

Figure . : The Fiber Display Dialog Box

The Fiber Display dialog box offers the same display options as those in the Fiber Mesh Display

dialog box (Figure . : The Fiber Mesh Display Dialog Box (p. )). Similarly, for the injections selected

in the Fiber Injections selection list, you can display either all injection fibers or single fibers with a

specified Fiber ID (when the Show Single Fiber option is selected).

You can color the fibers by the fiber variables listed in XY Plots (p. ) or by the following additional

fiber variables:

Fiber ID

Fiber Density

Fiber Tension

You can control the smooth gradation of fiber colors by specifying the number of fiber Levels.

The Fiber Module can be used in serial as well as in parallel calculations. Simulations in parallel require

no additional input. The fiber iterations are performed entirely on the host process, whereas the flow

field is parallelized. As a result, the overall performance may be limited by the host process if the fiber

calculations are more time-consuming than the parallel flow-field iterations. Therefore, when simulating

a large number of fibers, it is recommended to spawn the host process on a suitable machine. Refer

to Parallel Processing in the Fluent User's Guide (p. ) for further information on how to set up parallel

calculations.

Chapter : Creating Reduced Order Models (ROMs)

You can use a stand-alone Fluent session to define a reduced order model (ROM) for production in the

ANSYS Workbench environment (through ANSYS DesignXplorer). The produced ROM can then be con-

sumed in the ROM Viewer.

You can create a ROM from a series of 2D or 3D simulations. The ROM is a mathematical approximation

of your full model, where you can change some inputs and get the solution immediately. These inputs

are defined as input parameters in ANSYS Fluent and can be material properties, inlet velocities, pressures

and so on.

The process of creating and analyzing ROMs can be broken into two parts:

ROM Production—You can setup a ROM case in stand alone Fluent and read this case into Fluent in Work-

bench, as described in Defining a ROM (p. ) and ROM Production in the DesignXplorer User's Guide.

ROM Consumption—The produced ROM can be consumed in the ROM Viewer (ROM Consumption in the

DesignXplorer User's Guide).

To learn more about ROMs, refer to Using ROMs in the DesignXplorer User's Guide.

.. Defining a ROM

Important

For release  R3, ROMs are only applicable for steady-state, Newtonian fluids without

shock waves (Ma<) or radiation.

Building a ROM in Fluent:

. Enable the ROM addon module by entering define/models/addon-module/ in the Fluent console.

. Initialize the case or read a data file.

Solution → Initialization → Initialize

. Create input parameters for the quantities of interest for the ROM.

You can choose any input parameters that you are interested in. Later, in the 3D ROM system, you can

deselect input parameters if you decide that there are parameters that you no longer want to vary. Note

that if you pick too many input parameters you may require additional snapshots to maintain accuracy

with the ROM. Refer to Creating a New Parameter (p. ) for additional information on creating input

Note

General guidance on the number of input parameters defined:

Low:  to

Medium:  to

High: more than

Very high: more than

. Create at least one output parameter.

The output parameter has no impact on the ROM, but you can use it to monitor the results while the

design points are being updated in ANSYS DesignXplorer. Refer to Creating Output Parameters (p. )

for additional information on output parameters.

. Enable the Reduced Order Model.

Setup → Models

Reduced Order Model → Edit...

Figure . : The Reduced Order Model Dialog Box

. Select your desired Variables and Zones and click Add>>. Any Custom Field Functions (p. ) that you have

defined are available for selection.

You can remove items from the Selected for ROM list by selecting them and clicking Delete.

Important

You are free to select all of the variables and zones that you are interested in, however, be

aware that if you select too many variables/zones, you will end up with bigger files.This is

Creating Reduced Order Models (ROMs)

especially true if you have a larger model. For particularly large models, you may want to select

smaller zones that adequately capture the physics of interest.

You must select the variables that correspond or are associated with the input and output

parameters that you have defined. For example, if you have Mass Flow Rate selected as an

output parameter, then you must have Velocity selected in the Variable list (because mass

flow rate = density * area * velocity).

. Review the selections you have made in the Selected for ROM list and click OK to confirm.

.. Reduced Order Model (ROM) Evaluation in Fluent

Apart from viewing results in the ROM Viewer, you may want to quickly visualize the results directly

within Fluent, which you can do when you are running Fluent in Workbench.

From within Fluent you can view:

Contours

Vectors

Pathlines

XY Plots

Surface and volume integral reports

To evaluate a ROM in Fluent:

. In Workbench, generate the romz file by right-clicking the ROM Builder cell and selecting Export ROM.

Save the romz file to your desired location.

Reduced Order Model (ROM) Evaluation in Fluent

. Right-click the Fluent Setup cell, and select Import ROM → Browse, to open the Select File dialog box

and import the romz file.

. Generate the solution in Fluent by clicking Update Project in the toolbar.

. Launch Fluent by double-clicking the Solution cell.

. Open the Reduced Order Model dialog box.

→ Setup → Models → ROM

Edit...

. Click the Evaluate tab. Here you can see all of the parameters used in creating the ROM.The range of acceptable

inputs is listed to the right of each variable.

. Enter a value for the variable you want evaluated (within the allowed range) and click Evaluate.

You can visually postprocess ROM variables using contour plots, vector plots, and so on.

. Open the Contours dialog box.

→ Results → Graphics → Contours

New...

. Ensure that Node Values are disabled. ROMs are evaluated at cell centers.

. Select ROM Cell Functions... from the Contours of drop-down list.

Note

The ROM Cell Functions... option is only available after you click Evaluate in the Evaluate

tab of the Reduced Order Model dialog box.

. Select the ROM variable that you want to visualize from the second Contours of drop-down list.

. Select the surfaces where you want to visualize the specified ROM variable. The list of available surfaces is

filtered to show only the surfaces where the ROM is evaluated, as defined during ROM setup.

. Click Save/Display.

The following limitations apply to postprocessing reduced order models in Fluent:

You cannot continue with the ROM solution after evaluating it.

Exporting solution data/variables will not include ROM snapshot data.

Flux and Force Reports are not available for ROM evaluated variables using ROM data.

Output parameters are not updated for Design of Experiments when the ROM is being evaluated in Fluent.

.. ROM Limitations

The following list of limitations should be viewed in conjunction with the list of limitations provided in

the ANSYS DesignXplorer documentation (ROM Limitations and Known Issues in the DesignXplorer User's

Guide):

You must have at least one input and one output parameter defined before you can enable the reduced

order model in Fluent.

Guide):

Polyhedral meshes are supported in the ROM Viewer, however they will be displayed with triangles. Note

that this does not affect the results.

The ROM Viewer does not support displaying results on edges—it can only display results on elements and

faces.

Interface zones are not available for use with ROMs.

The 3D ROM does not support geometry parameter updates.

ROMs can only be created for steady-state cases.

Combustion and radiation models are not supported for ROMs.

Parametric optimization using the ROM through Fluent is not supported.

ROM Limitations

Moving and deforming meshes are not supported for ROMs.

You must select the variables that correspond with the input and output parameters that you have defined.

Contours in Fluent and the ROM Viewer:While contour displays may appear similar in Fluent and the ROM

Viewer, there are some key differences in how they display data that could appear to show inconsistencies

that are not actually present in the results. In Fluent, contours are displayed using node values (by default)

or cell-center values if node values are disabled. In contrast, the ROM Viewer displays contours using face

values (not an option in Fluent). In most cases, node values can appear very comparable to face values, but

there are some instances where that is not the case.

Chapter : Using the Solver

This chapter describes how to use the ANSYS Fluent solver. For more information about the theory

behind the ANSYS Fluent solver, see Solver Theory in the Theory Guide. Choosing the Solver (p. )

provides an overview, and the remaining sections provide detailed instructions.

.. Overview of Using the Solver

.. Choosing the Spatial Discretization Scheme

.. Pressure-Based Solver Settings

.. Density-Based Solver Settings

.. Setting Algebraic Multigrid Parameters

.. Setting Solution Limits

.. Setting Multi-Stage Time-Stepping Parameters

.. Selecting Gradient Limiters

.. Full Multigrid (FMG) Initialization

.. Hybrid Initialization

.. Performing Steady-State Calculations

.. Performing Pseudo Transient Calculations

.. Performing Time-Dependent Calculations

.. Monitoring Solution Convergence

.. Convergence Conditions

.. Executing Commands During the Calculation

.. Automatic Initialization of the Solution and Case Modification

.. Animating the Solution

.. Checking Your Case Setup

.. Convergence and Stability

.. Solution Steering

In ANSYS Fluent, two solver technologies are available:

pressure-based

density-based

Both solvers can be used for a broad range of flows, but in some cases one formulation may perform

better (that is, yield a solution more quickly or resolve certain flow features better) than the other. The

pressure-based and density-based approaches differ in the way that the continuity, momentum, and

(where appropriate) energy and species equations are solved, as described in Overview of Flow Solvers

The pressure-based solver traditionally has been used for incompressible and mildly compressible flows.

The density-based approach, on the other hand, was originally designed for high-speed compressible

flows. Both approaches are now applicable to a broad range of flows (from incompressible to highly

compressible), but the origins of the density-based formulation may give it an accuracy (that is shock

resolution) advantage over the pressure-based solver for high-speed compressible flows.

Two formulations exist under the density-based solver: implicit and explicit. The density-based explicit

and implicit formulations solve the equations for additional scalars (for example, turbulence or radiation

quantities) sequentially. The implicit and explicit density-based formulations differ in the way that they

linearize the coupled equations. For more details about the solver formulations, see Overview of Flow

Solvers in the Theory Guide.

Due to broader stability characteristics of the implicit formulation, a converged steady-state solution

can be obtained much faster using the implicit formulation rather than the explicit formulation. However,

the implicit formulation requires more memory than the explicit formulation.

Two algorithms also exist under the pressure-based solver in ANSYS Fluent: a segregated algorithm and

a coupled algorithm. In the segregated algorithm the governing equations are solved sequentially, se-

gregated from one another, while in the coupled algorithm the momentum equations and the pressure-

based continuity equation are solved in a coupled manner. In general, the coupled algorithm significantly

improves the convergence speed over the segregated algorithm, however, the memory requirement

for the coupled algorithm is more than the segregated algorithm.

When selecting a solver and an algorithm you must consider the following issues:

The model availability for a given solver.

Solver performance for the given flow conditions.

The size of the mesh under consideration and the available memory on your machine.This issue could be

an important factor in deciding whether to use an explicit or implicit formulation when the density-based

solver is selected, or to use a segregated or coupled algorithm when the pressure-based solver is selected.

The following two lists highlight the model availability for each solver:

Important

Note that the pressure-based solver provides several physical models or features that are

not available with the density-based solver:

Cavitation model

Volume-of-fluid (VOF) model

Multiphase mixture model

Eulerian multiphase model

Non-premixed combustion model

Premixed combustion model

Partially premixed combustion model

Composition PDF transport model

Soot model

Rosseland radiation model

Using the Solver

Shell conduction model

Floating operating pressure

Fixed variable option

Physical velocity formulation for porous media

Specified mass flow rate for streamwise periodic flow

The following features are available with the density-based solver, but not with the pressure-based

solver:

Wet steam multiphase model

... Choosing the Solver

To choose one of the solvers, you will use the General Task Page (p. ) (Figure . : The General Task

Page (p. )).

Setup →

General

Figure . : The General Task Page

Setup →

General

Overview of Using the Solver

To use the pressure-based solver, retain the default selection of Pressure-Based under Solver.

To use the density-based solver, select Density-Based under Solver.

After you have defined your model and specified which solver you want to use, you are ready to run

the solver. The following steps outline a general procedure you can follow:

. (pressure-based solver only) Select the pressure-velocity coupling method (see Choosing the Pressure-

Velocity Coupling Method (p. )).

. Choose the spatial discretization scheme and, for the pressure-based solver, the pressure interpolation

scheme (see Choosing the Spatial Discretization Scheme (p. )).

. (pressure-based solver only) Select the porous media velocity method (see Porous Media Conditions (p. )).

. Select how you want the derivatives to be evaluated by choosing a gradient option (see Evaluation of

Gradients and Derivatives in the Theory Guide).

. Set the under-relaxation factors (see Setting Under-Relaxation Factors (p. )).

. (density-based explicit formulation only) Set up the FAS multigrid (see Turning On FAS Multigrid (p. )).

. Make any additional modifications to the solver settings that are suggested in the chapters or sections

that describe the models you are using.

. Enable the appropriate solution monitors (see Monitoring Solution Convergence (p. )).

. Initialize the solution (see Initializing the Solution (p. )).

. Start calculating (see Performing Steady-State Calculations (p. ) for steady-state calculations, or Perform-

ing Time-Dependent Calculations (p. ) for time-dependent calculations).

. If you have convergence trouble, try one of the methods discussed in Convergence and Stability (p. ).

The default settings for the first three items listed above are suitable for most problems and need not

be changed. The following sections outline how these and other solution parameters can be changed,

and when you may want to change them.

Gradients are needed not only for constructing values of a scalar at the cell faces, but also for computing

secondary diffusion terms and velocity derivatives. For more information about the different gradients,

see Evaluation of Gradients and Derivatives in the Theory Guide.

The three gradients that are available in ANSYS Fluent are

Green-Gauss Cell Based

Green-Gauss Node Based

Least Squares Cell Based

The gradient options are selectable from the Gradient drop-down list, in the Solution Methods task

page.

Solution →

Methods

In addition, ANSYS Fluent allows you to choose the discretization scheme for the convection terms of

each governing equation. (Second-order accuracy is automatically used for the viscous terms.) By default,

single-phase problems using either the pressure-based or density-based solver are solved using second-

order upwind discretization for the convection terms of the flow equations and all scalar equations

except those for turbulence quantities, which are solved using first-order upwind discretization. For

multiphase flows, the flow equations use first-order upwind discretization by default. For a complete

description of the discretization schemes available in ANSYS Fluent, see Discretization in the Theory

Guide.

In addition, when you use the pressure-based solver, you can specify the pressure interpolation scheme.

For a description of the pressure interpolation schemes available in ANSYS Fluent, see Pressure Interpol-

ation Schemes in the Theory Guide.

... First-Order Accuracy vs. Second-Order Accuracy

... Other Discretization Schemes

... Choosing the Pressure Interpolation Scheme

... Choosing the Density Interpolation Scheme

... High Order Term Relaxation (HOTR)

When the flow is aligned with the mesh (for example, laminar flow in a rectangular duct modeled with

a quadrilateral or hexahedral mesh) the first-order upwind discretization may be acceptable. When the

flow is not aligned with the mesh (that is, when it crosses the mesh lines obliquely), however, first-

order convective discretization increases the numerical discretization error (numerical diffusion). For

triangular and tetrahedral meshes, since the flow is never aligned with the mesh, you will generally

obtain more accurate results by using the second-order discretization. For quad/hex meshes, you will

also obtain better results using the second-order discretization, especially for complex flows.

In summary, while the first-order discretization generally yields better convergence than the second-

order scheme, it generally will yield less accurate results, especially on tri/tet meshes. See Convergence

and Stability (p. ) for information about controlling convergence.

For most cases, you will be able to use the second-order scheme from the start of the calculation. In

some cases, however, you may need to start with the first-order scheme and then switch to the second-

order scheme after a few iterations. For example, if you are running a high-Mach-number flow calculation

that has an initial solution much different than the expected final solution, you will usually need to

perform a few iterations with the first-order scheme and then turn on the second-order scheme and

continue the calculation to convergence. Alternatively, full multigrid initialization is also available for

some flow cases that allow you to proceed with the second-order scheme from the start.

For a simple flow that is aligned with the mesh (for example, laminar flow in a rectangular duct modeled

with a quadrilateral or hexahedral mesh), the numerical diffusion will be naturally low, so you can

generally use the first-order scheme instead of the second-order scheme without any significant loss

of accuracy.

Finally, if you run into convergence difficulties with the second-order scheme, you should try the first-

order scheme instead.

Choosing the Spatial Discretization Scheme

.... First- to Higher-Order Blending

While the higher-order scheme may result in greater accuracy, it can also result in convergence diffi-

culties and instabilities at certain flow conditions. On the other hand, using a first-order scheme may

not provide the desired accuracy. One approach to achieving improved accuracy while maintaining

good stability is to use a discretization blending factor. This feature is available for both density-based

and pressure-based solvers and can be invoked using the following text command:

Enter a value between  and  when asked for the blending factor: 1st-order to higher-order

blending factor [min=. - max=.]

A blending factor of  reduces the gradient reconstruction to a first-order discretization scheme,

whereas  will recover high-order discretization. A blending factor of less than  (typically . or

.) will make the convective fluxes more diffusive, which in some flow conditions can stabilize a

solution that is otherwise unstable when the full higher-order discretization scheme is employed.

Important

Note that in order to use this feature effectively, make sure that one of the allowed higher-

order discretization schemes is selected for the desired variables in the Solution Methods

task page.

The QUICK and third-order MUSCL discretization schemes may provide better accuracy than the second-

order scheme for rotating or swirling flows. The QUICK scheme is applicable to quadrilateral or hexa-

hedral meshes, while the MUSCL scheme is used on all types of meshes. In general, however, the

second-order scheme is sufficient and the QUICK scheme will not provide significant improvements

in accuracy.

Important

Important

If QUICK is used for hybrid meshes, it will be used only for quadrilateral and hexahedral

cells. Second-order upwind discretization will be applied to all other cells.

The bounded central differencing and (for the pressure-based solver) central differencing schemes are

available when you are using the LES, DES, SAS, SBES, and SDES turbulence models, and the central

differencing scheme should be used only when the mesh spacing is fine enough so that the magnitude

of the local Peclet number (see Equation . in the Theory Guide) is less than .

A modified HRIC scheme (see Modified HRIC Scheme in the Theory Guide) is also available for VOF

simulations using either the implicit or explicit formulation.

As discussed in Pressure Interpolation Schemes in the Theory Guide, a number of pressure interpolation

schemes are available when the pressure-based solver is used in ANSYS Fluent. For most cases the

second-order scheme is acceptable, but some types of models may benefit from one of the other

schemes:

For mixture or VOF multiphase models, either the PRESTO! or body-force-weighted schemes should be

used and only these schemes are made available.The default in these cases is PRESTO!.

For Eulerian multiphase models, the default scheme is PRESTO!. However, for multi-fluid VOF problems

that use the non-iterative solver, the Second Order interpolation scheme can be more robust for cases

with skewed meshes, and the Body Force Weighted interpolation scheme can be more robust for cases

with large body forces and skewed meshes.

For problems involving large body forces, the body-force-weighted scheme is recommended.

For flows with high swirl numbers, high-Rayleigh-number natural convection, high-speed rotating flows,

and flows in strongly curved domains, use the PRESTO! scheme.

As discussed in Density Interpolation Schemes in the Theory Guide, four density interpolation schemes

are available when the pressure-based solver is used to solve a single-phase compressible flow.

The second-order upwind scheme (the default) provides reasonable stability for the discretization of

the pressure-correction equation, and gives good results for most classes of flows. The first-order upwind

scheme will provide greater stability, but may tend to smooth shocks in compressible flows. If you are

calculating a compressible flow with shocks you should use the second-order-upwind or QUICK scheme.

Using the QUICK scheme for all variables, including density, is highly recommended for compressible

flows with shocks when using quadrilateral, hexahedral, or hybrid meshes. The third-order MUSCL

scheme is applicable to arbitrary meshes and has the potential to improve spatial accuracy for all types

of meshes by reducing numerical diffusion.

Important

In the case of multiphase flows, the selected density scheme is applied to the compressible

phase and arithmetic averaging is used for incompressible phases.

The purpose of the relaxation of high order terms is to improve the startup and the general solution

behavior of flow simulations when higher order spatial discretizations are used (higher than first). It

has also shown to prevent convergence stalling in some cases. Such high-order terms can be of signi-

ficant importance in certain cases and lead to numerical instabilities. This is particularly true at aggressive

solution settings. In such cases, high order relaxation is a useful strategy to minimize your interaction

during the solution. This can be an effective alternative to starting the solution first order, then

switching to second order spatial discretization at a later stage.

The High Order Term Relaxation option can be enabled from the Solution Methods task page, as

shown in Figure . : The Solution Methods Task Page for the HOTR Option (p. ).

Solution →

Methods

Figure . : The Solution Methods Task Page for the HOTR Option

Further control of High Order Term Relaxation can be obtained after clicking Options... and making

the necessary selections and settings in the Relaxation Options dialog box (Figure . : The Relaxation

Figure . : The Relaxation Options Dialog Box

You have the option of selecting All Variables to be under-relaxed instead of only the default flow

variables (Flow Variables Only).

If you select Flow Variables Only, then the following variables will be under-relaxed:

– Velocity components

– Pressure

– Energy

– Density

– Turbulence quantities (excluding Reynolds stresses)

– Volume fraction

If you select All Variables, then relaxation is applied to each variable discretized with a higher order

– Density

scheme.

The default values for the Relaxation Factor is . for steady-state cases and . for transient cases.

The same factor is applied to all equations solved.

For theoretical information about high order term relaxation, see High Order Term Relaxation in the

The following limitations exist when using the High Order Term Relaxation option:

The High Order Term Relaxation option is not available when the Non-Iterative Time Advancement

option is enabled, since the simulation would not achieve the required level of high order spatial

accuracy.

In general, high order term relaxation is available for transient flows. Nevertheless, it should be used

with care.To achieve high order accuracy at convergence for each time step, you must increase the

number of iterations per time step to ensure that the original convergence criteria have been met.

When the QUICK scheme is selected for specific transport equations, no under-relaxation is applied

to this equation.

You can specify the discretization scheme and, for the pressure-based solver, the pressure interpolation

scheme in the Solution Methods Task Page (p. ) (Figure . : The Solution Methods Task Page for

the Pressure-Based Segregated Algorithm (p. )).

Solution →

Methods

Figure . : The Solution Methods Task Page for the Pressure-Based Segregated Algorithm

For each scalar equation listed under Spatial Discretization (Momentum, Energy, Turbulent Kinetic

Energy, and so on, for the pressure-based solver or Turbulent Kinetic Energy, Turbulent Dissipation

Rate, and so on, for the density-based solver) you can choose First Order Upwind, Second Order

Upwind, QUICK, Third-Order MUSCL, or (for Momentum when you are using the LES, DES, SAS, SDES,

or SBES turbulence model) Bounded Central Differencing (the default) or Central Differencing in

the adjacent drop-down list. For the density-based solver, you can choose either First Order Upwind,

Second Order Upwind, Third-Order MUSCL, or (when you are using the LES, DES, SAS, SDES, or SBES

turbulence model) Bounded Central Differencing for the Flow equations (which include momentum

and energy). Note that the task page shown in Figure . : The Solution Methods Task Page for the

Pressure-Based Segregated Algorithm (p. ) is for the pressure-based solver.

If you are using the pressure-based solver, select the pressure interpolation scheme under Spatial

Discretization, in the drop-down list next to Pressure. You can choose Standard, PRESTO!, Linear,

Second Order, or Body Force Weighted.

Important

The low-order formulation of PRESTO! can be applied by limiting the high-order terms for

the PRESTO! scheme. This is done using the following text command:

When asked limit high-order terms for PRESTO! pressure scheme?, enter

yes.

This modification can be used to stabilize the solution process when the pressure-based

coupled algorithm is used and when the original PRESTO! scheme either fails to converge

or produces unphysical oscillations (wiggles) in the pressure field.

If you are using the pressure-based solver and your flow is compressible (that is, you are using the

ideal gas law for density), select the density interpolation scheme under Spatial Discretization, in the

drop-down list next to Density. You can choose First Order Upwind, Second Order Upwind, QUICK

or Third-Order MUSCL. (Note that Density will not appear for incompressible flows.)

If you enable the VOF model while using the pressure-based solver, the volume fraction interpolation

schemes that are available are Geo-Reconstruct, CICSAM, Modified HRIC, and QUICK.

If your case involves species transport, you can set the scheme for the individual species as First Order

Upwind, Second Order Upwind, QUICK, or Third-Order MUSCL. However, if you want all your species

to use the same discretization scheme, then rather than setting each one individually, simply enable

the Set All Species Discretizations Together option. Notice that you will no longer see your list of

individual species, instead a Species field will appear with the scheme of your choice.

If you change the settings for the Spatial Discretization, but you then want to return to ANSYS Fluent’s

default settings, you can click the Default button.

Important

If your mesh topology has step-wise prism mesh near the walls, do not use node-based

gradients with MUSCL.

... Choosing the Pressure-Velocity Coupling Method

... Setting Under-Relaxation Factors

... Setting Solution Controls for the Non-Iterative Solver

... Equation Order

The pressure-velocity coupling scheme controls the manner in which pressure and velocity are updated

when the pressure-based solver is used. The scheme can be either segregated (pressure and velocity

are updated sequentially) or coupled (pressure and velocity are updated simultaneously).

ANSYS Fluent provides the following segregated types of algorithms:

SIMPLE

SIMPLEC

PISO

Fractional Step (FSM) (time-dependent flows with Non-Iterative Time Advancement (NITA) only)

In general, segregated methods are faster per iteration, while the coupled algorithm usually requires

fewer iterations to converge. For this reason, the coupled solver is usually recommended for steady-

state simulations. For transient simulations, the coupled solver has the best robustness properties, es-

pecially for large time step sizes, but SIMPLEC, PISO, or NITA may give faster overall solution times for

small time step sizes.

The coupled solver offers the following mechanisms to under-relax the equations:

Pseudo Transient (steady-state only)

Courant number

Coupled pseudo-transient is the default selection for cases with the following settings:

Steady-state

Single-phase

No battery or fuel cell model

No solidification and melting model

Controls for the coupled pseudo-transient solver are described in Performing Pseudo Transient Calcu-

lations (p. ). The most important (and typically the only) control you need to adjust in practice is

the Pseudo Time Step, as described in Solving Pseudo-Transient Flow (p. ).

Important

Important

Pressure-velocity coupling is relevant only for the pressure-based solver.

.... SIMPLE vs. SIMPLEC

In ANSYS Fluent, both the standard SIMPLE algorithm and the SIMPLEC (SIMPLE-Consistent) algorithm

are available. SIMPLE is the default, but many problems will benefit from using SIMPLEC, particularly

because of the increased under-relaxation that can be applied, as described below.

For relatively uncomplicated problems (laminar flows with no additional models enabled) in which

convergence is limited by the pressure-velocity coupling, you can often obtain a converged solution

more quickly using SIMPLEC. With SIMPLEC, the pressure-correction under-relaxation factor is generally

set to ., which aids in convergence speed-up. In some problems, however, increasing the pressure-

correction under-relaxation to . can lead to instability due to high mesh skewness. For such cases,

you will need to use one or more skewness correction schemes, use a slightly more conservative under-

relaxation value (up to . ), or use the SIMPLE algorithm. For complicated flows involving turbulence

and/or additional physical models, SIMPLEC will improve convergence only if it is being limited by

the pressure-velocity coupling. Often it will be one of the additional modeling parameters that limits

convergence; in this case, SIMPLE and SIMPLEC will give similar convergence rates.

.... PISO

The PISO algorithm (see PISO in the Theory Guide) with neighbor correction is highly recommended

.... PISO

for all transient flow calculations, especially when you want to use a large time step. (For problems

that use the LES turbulence model, which usually requires small time steps, using PISO may result in

an increased computational expense, so SIMPLE or SIMPLEC should be considered instead.) PISO can

maintain a stable calculation with a larger time step and an under-relaxation factor of . for both

momentum and pressure. For steady-state problems, PISO with neighbor correction does not provide

any noticeable advantage over SIMPLE or SIMPLEC with optimal under-relaxation factors.

PISO with skewness correction is recommended for both steady-state and transient calculations on

meshes with a high degree of distortion.

When you use PISO neighbor correction, under-relaxation factors of . or near . are recommended

for all equations. If you use just the PISO skewness correction for highly-distorted meshes (without

neighbor correction), set the under-relaxation factors for momentum and pressure so that they sum

to  (for example, . for pressure and . for momentum). If you use both PISO methods, follow the

under-relaxation recommendations for PISO neighbor correction, above.

For most problems, it is not necessary to disable the default coupling between neighbor and skewness

corrections. For highly distorted meshes, however, disabling the default coupling between neighbor

and skewness corrections is recommended.

.... Fractional Step Method

The Fractional Step method (FSM), described in Fractional-Step Method (FSM) in the Theory Guide,

is available when you choose to use the NITA scheme (that is, the Non-Iterative Time Advancement

option in the Solution Methods task page). With the NITA scheme, the FSM is slightly less computa-

tionally expensive compared to the PISO algorithm. Whether you select FSM or PISO depends on the

application. For some problems (for example, simulations that use VOF), FSM could be less stable

than PISO.

In most cases, the default values for the solution methods are enough to set a robust convergence

of the internal pressure correction sub-iterations due to skewness. Only very complex problems (for

example, moving deforming meshes, sliding interfaces, the VOF model) could require a reduction of

relaxation for pressure up to a value of . or ..

.... Coupled

Selecting Coupled from the Pressure-Velocity Coupling drop-down list indicates that you are using

the pressure-based coupled algorithm, described in Coupled Algorithm in the Theory Guide. This

Pressure-Based Solver Settings

solver offers some advantages over the pressure-based segregated algorithm. The pressure-based

coupled algorithm obtains a more robust and efficient single phase implementation for steady-state

flows. It is not available for cases using the Non-Iterative Time Advancement option (NITA).

Note

In some cases using porous jump boundary conditions, the Coupled scheme may suffer

from convergence issues that do not respond to changes in the coupled solver settings.

This behavior depends on the specific flow configuration and porous jump boundary

condition values. If convergence instability is observed in cases using porous jump

boundary conditions and the Coupled scheme, it is recommended that you change the

pressure-velocity coupling to one of the segregated schemes.

.... User Inputs

You can specify the pressure-velocity coupling method in the Solution Methods Task Page (p. )

(Figure . : The Solution Methods Task Page for the Pressure-Based Segregated Algorithm (p. )).

Solution →

Methods

Choose SIMPLE, SIMPLEC, PISO, Fractional Step, or Coupled in the Pressure-Velocity Coupling

If you choose PISO, the task page will expand to show the additional parameters for pressure-velocity

coupling. By default, the number of iterations for Skewness Correction and Neighbor Correction

are set to . If you want to use only Skewness Correction, then set the number of iterations for

Neighbor Correction to . Likewise, if you want to use only Neighbor Correction, then set the

number of iterations for Skewness Correction to . For most problems, you do not need to change

the default iteration values. By default, the Skewness-Neighbor Coupling option is enabled to allow

for a more economical, but a less robust variation of the PISO algorithm.

If you choose SIMPLEC under Pressure-Velocity Coupling, you must also set the Skewness Correc-

tion, whose default value is .

If you choose Coupled without the Pseudo Transient option, you will have to specify the Courant

number in the Solution Controls task page, which is set at  by default. You will also specify the

Explicit Relaxation Factors for Momentum and Pressure, which are set at . by default. For more

information about these options, refer to Pressure-Velocity Coupling and Steady-State Iterative Al-

gorithm in the Theory Guide.

For cases with very skewed meshes, the run can be stabilized by further reduction of the explicit re-

laxation factor to .. If ANSYS Fluent immediately diverges in the AMG solver, then the CFL number

is too high and should be reduced. Reducing the CFL number below  is not recommended since

it would be better to use the segregated algorithm for the pressure-velocity coupling.

In most transient cases, the CFL number should be set to a large value such as  and explicit relax-

ation factors to ..

If you choose Coupled and enable the Pseudo Transient option, you will set the Pseudo Transient

Explicit Relaxation Factors in the Solution Controls task page, as described in Setting Pseudo

Transient Explicit Relaxation Factors (p. ).

The pressure-based solver uses under-relaxation of equations to control the update of computed

variables at each iteration (as described in Under-Relaxation of Equations in the Theory Guide). This

means that all equations solved using the pressure-based solver, including the non-coupled equations

solved by the density-based solver (turbulence and other scalars, as discussed in Density-Based Solver

in the Theory Guide), will have under-relaxation factors associated with them.

In ANSYS Fluent, the default under-relaxation parameters for all variables are set to values that are

near optimal for the largest possible number of cases. These values are suitable for many problems,

but for some particularly nonlinear problems (for example, some turbulent flows or high-Rayleigh-

number natural-convection problems) it is prudent to reduce the under-relaxation factors initially.

It is good practice to begin a calculation using the default under-relaxation factors. If the residuals

continue to increase after the first  or  iterations, you should reduce the under-relaxation factors.

Occasionally, you may make changes in the under-relaxation factors and resume your calculation, only

to find that the residuals begin to increase. This often results from increasing the under-relaxation

factors too much. A cautious approach is to save a data file before making any changes to the under-

relaxation factors, and to give the solution algorithm a few iterations to adjust to the new parameters.

Typically, an increase in the under-relaxation factors brings about a slight increase in the residuals, but

these increases usually disappear as the solution progresses. If the residuals jump by a few orders of

magnitude, you should consider halting the calculation and returning to the last good data file saved.

Note that viscosity and density are under-relaxed from iteration to iteration. Also, if the enthalpy

equation is solved directly instead of the temperature equation (that is, for non-premixed combustion

calculations), the update of temperature based on enthalpy will be under-relaxed. To see the default

under-relaxation factors, you can click the Default button in the Solution Controls Task Page (p. ).

For most flows, the default under-relaxation factors do not usually require modification. If unstable or

divergent behavior is observed, however, you need to reduce the under-relaxation factors for pressure,

momentum,

, and  from their default values to about ., ., ., and .. (It is usually not necessary

to reduce the pressure under-relaxation for SIMPLEC.) In problems where density is strongly coupled

with temperature, as in very-high-Rayleigh-number natural- or mixed-convection flows, it is wise to

also under-relax the temperature equation and/or density (that is, use an under-relaxation factor less

than . ). Conversely, when temperature is not coupled with the momentum equations (or when it is

weakly coupled), as in flows with constant density, the under-relaxation factor for temperature can be

set to ..

For other scalar equations (for example, swirl, species, mixture fraction and variance) the default under-

relaxation may be too aggressive for some problems, especially at the start of the calculation. You may

want to reduce the factors to . to facilitate convergence.

You can modify the under-relaxation factors in the Solution Controls Task Page (p. ) (Figure . : The

Solution Controls Task Page for the Pressure-Based Solver (p. )).

Solution →

Controls

Figure . : The Solution Controls Task Page for the Pressure-Based Solver

Solution →

Controls

You can set the under-relaxation factor for each equation in the field next to its name under Under-

Relaxation Factors.

Important

If you are using the pressure-based solver, all equations will have an associated under-re-

laxation factor (see Under-Relaxation of Equations in the Theory Guide). If you are using

the density-based solver, only those equations that are solved sequentially (see Density-

Based Solver in the Theory Guide) will have under-relaxation factors.

If your case involves species transport, you can set the under-relaxation factors for each of the listed

species. If you want all your species to use the same under-relaxation factors, simply enable the Set

All Species URFs Together option. Notice that you will no longer see your list of individual species,

instead a Species field will appear where you will specify the under-relaxation factor.

If you change under-relaxation factors, but you then want to return to ANSYS Fluent’s default settings,

you can click the Default button.

Note that with optimal settings, the convergence of the coupled pressure-velocity algorithm will be

limited by the segregated solution of other scalar equations, for example, turbulence. For optimum

solver performance, you will need to increase the relaxation factors for these equations to a value

greater than the default values.

You can use the non-iterative solver (see Time-Advancement Algorithm in the Theory Guide) for tran-

sient problems in order to increase the speed and efficiency of the calculations. You can also obtain

a steady solution using the non-iterative multiphase solver for multiphase flows with quasi-steady

To control the change of computed variables at each iteration, you can specify explicit relaxation in

the Non-Iterative Solver Relaxation Factors list in the Solution Controls Task Page (p. ). Additional

information on relaxation factors can be found in Setting Under-Relaxation Factors (p. ).

Other solution controls are accessible via the Expert tab, in the Advanced Solution Controls dialog

box (see Figure . : The Advanced Solution Controls Dialog Box for the Pressure-Based Segregated

Non-Iterative Solver (p. )). The criteria for convergence include the Correction Tolerance (defined

by the overall accuracy), Residual Tolerance (controlling the solution of the linear equations), and

Max. Corrections (controlling the maximum number of sub-iterations for each individual equation).

The default control settings are optimally designed in order to get a second-order accurate solution.

To use ANSYS Fluent’s non-iterative transient solver in order to boost the efficiency of transient simu-

lations:

. Go to the Solution Methods task page.

Solution →

Methods

. Make sure that Coupled is not selected from the Pressure-Velocity Coupling drop-down list.

. Enable Non-Iterative Time Advancement.

. Under Pressure-Velocity Coupling, select a scheme from the drop-down list:

For single phase or VOF multiphase flows:You can select either the Fractional Step or PISO scheme.

For the PISO scheme, you can set the value for the Neighbor Correction. Skewness correction is per-

formed automatically.

For Eulerian multiphase flows: Select the Phase Coupled SIMPLE.This is the only pressure scheme

available for NITA multiphase simulations.

. When using the Large Eddy Simulation (LES) turbulence model, you can enable the Accelerated

Time Marching option in order to speed up the simulation. This option is intended for unreacting

flow simulations that use a constant-density fluid. It enables a modified NITA scheme and changes

the following to a more aggressive setting:

The maximum number of sub-iterations for the NITA solver equations (specified in the Expert tab of

the Advanced Solution Controls dialog box) are revised: the Max. Corrections is set to  for Pressure

and  for all other equations.

The pressure-velocity coupling scheme (specified in the Solution Methods task page) is changed to

the Fractional Step method.

The multigrid solver settings (specified in the Multigrid tab of the Advanced Solution Controls dialog

box) are revised: for the Pressure equation, the Cycle Type is changed to F-Cycle and the Termination

criterion is set to ..

Note

The following limitations / recommendations apply:

The accelerated time marching option is not available with the Eulerian multiphase model.

It is not recommended for compressible or variable-density fluids.

When using this option, it is recommended that you use the Bounded Central Differencing

scheme for the Momentum equation rather than the Central Differencing scheme.

Solution →

Controls

The relaxation factors define the explicit relaxation (see Under-Relaxation of Variables in the Theory

Guide) of variables between sub-iterations. The relaxation factors can be used to prevent the solution

from diverging.

If the solution is unstable:

For single phase flows:You should first try to stabilize the solution by lowering the relaxation factors for

pressure to .–., and by reducing the time step.

For multiphase flows: Consider lowering the explicit pressure relaxation factor up to ..This may help

when meshes are poor, because a poor mesh will significantly affect the pressure gradient, which in turn

may generate large source terms in the governing equations resulting in poor convergence.You can set

the under-relaxation factors for the other flow variables to higher values (.-.). For compressible mul-

tiphase flow, you can use explicit relaxation of density in the range .-.. For multiphase cases with

mass transfer, you can use explicit relaxation of vaporization mass in the range .-..

You can modify the non-iterative solution controls in the Advanced Solution Controls Dialog Box (p. )

(Figure . : The Advanced Solution Controls Dialog Box for the Pressure-Based Segregated Non-Iter-

ative Solver (p. )).

Solution →

Solution →

Figure . : The Advanced Solution Controls Dialog Box for the Pressure-Based Segregated

Non-Iterative Solver

Under Non-Iterative Solver Controls, there are several parameters that control the sub-iterations

for the individual equations.

The sub-iterations for an equation stop when the total number of sub-iterations exceeds the value

specified for Max. Corrections, regardless of whether or not the convergence criteria (described below)

are met.

The sub-iterations for an equation end when the ratio of the residuals at the current sub-iteration

and the first sub-iteration is less than the value specified in the Correction Tolerance field. You can

monitor the details of the sub-iteration convergence by looking at the AMG solver performance (that

is, setting the Verbosity field in the Multigrid tab in the Advanced Solution Controls dialog box

to ). Be sure to pay attention to the residuals for the current sub-iteration (that is, the residual for

the -th AMG cycle at the current sub-iteration) and the initial residual of the time step (that is, the

residual for the -th AMG cycle of the first sub-iteration). The ratio of these two residuals is what is

controlled by the Correction Tolerance field. These two residuals are also the residuals plotted when

using the Residual Monitor panel and reported in the ANSYS Fluent console at the end of a time

step. Note that the residuals reported at the end of a time step can be scaled or unscaled, depending

on the settings in the Residual Monitor dialog box. The residuals reported when monitoring the

AMG solver performance are always unscaled.

For each interim sub-iteration, the AMG cycles continue until the usual AMG termination criteria (.

by default, and set in the Multigrid tab) are met. However, for the last sub-iteration (that is, either

when the maximum number of sub-iterations are reached or when the correction tolerance is satisfied),

the AMG cycles continue until the ratio of the residual at the current cycle to the initial residual (the

residual for the -th AMG cycle of the first sub-iteration of the time step) drops below the value

specified for Residual Tolerance. You may want to adjust the Residual Tolerance, depending on

the time step selected. The default Residual Tolerance should be well suited for moderate time steps

(that is, for cell CFL numbers of  to ). Note that you can display the cell CFL numbers for unsteady

problems by selecting Cell Courant Number in the Velocity... category of all postprocessing dialog

boxes. For very small time steps (cell CFL <<), the diagonal dominance of the system is very high

and the convergence should be driven further by reducing the Residual Tolerance value. For larger

time steps (cell CFL >>), it may be possible that the residual tolerance cannot be reached due to

round-off errors, and unless the Residual Tolerance value is increased, AMG cycles can be wasted.

Again, this can be monitored by monitoring the AMG solver performance.

.... NITA Expert Options

To obtain diagnostics on convergence of sub-iterations for individual equations, use the following text

command:

solve/set/nita-expert-controls/set-verbosity

verbosity []

command:

The output information may help you to judge whether the specified number of sub-iterations is

sufficient to reach the correction tolerance and also to diagnose the source of the solution diver-

gence.

For NITA cases with PISO selected as a Pressure-Velocity Coupling scheme, you can enable coupling of

the neighbor and skewness corrections with the following TUI command:

solve/set/nita-expert-controls/skewness-neighbor-coupling

enable skewness neighbor coupling for nita [no] yes

For more information about this option, see Skewness - Neighbor Coupling in the Fluent Theory

Guide.

For NITA cases that involve VOF, hybrid NITA expert options may help you to improve solution robustness,

but at the cost of speed. Depending on your case, the hybrid NITA expert settings may optimize NITA

expert controls, explicit relaxation factors, and outer iterations.To use the hybrid NITA expert options,

solve/set/nita-expert-controls/hybrid-nita-settings

enable hybrid nita settings? [no] yes

–  : Recommended for incompressible and Newtonian (low viscosity ratio) flow.

–  : Recommended for compressible and Newtonian (low viscosity ratio) flow and heat/mass-transfer.

–  : Recommended for non-Newtonian or high viscosity ratio flow.You can also use this option when

there is a strong equation coupling, and the above options do not produce useful results.

In case of divergence when using NITA, the following settings may help:

– Switch to a different pressure spatial discretization scheme (from PRESTO! to Body Force Weighted

or vice versa).

– Reduce Explicit Relaxation Factors for pressure, momentum and volume fraction down to ..

Note

Currently, the residual reports display two residuals for each outer iteration.

.... Compatibility of the NITA Scheme with Other ANSYS Fluent Models

The following is a list of models that are compatible with the non-iterative solver:

Inviscid flow (excluding ideal gas)

Laminar flow

All models of turbulence (including LES and DES)

S2S radiation model

Non-reacting species transport

General compressible flows (most subsonic and some transonic applications)

VOF multiphase model (most applications)

Phase change (solidification and melting)

Porous media model (isotropic resistance)

Multiphase model with Multi-Fluid VOF

Multiphase RSM turbulence model

The following is a list of models that are compatible with the non-iterative solver, but may result in

some instabilities and inaccuracies for certain flow conditions:

RSM turbulence model

MDM

Non-Newtonian fluids

General compressible flows (aerospace supersonic applications)

Reacting species and any type of combustion including PDF

The following is a list of models that are not compatible with the non-iterative solver:

Mixture model

Radiation models (except S2S)

DPM, spark, and crevice models

UDS transport

Porous jump

Porous media model (anisotropic resistance)

Important

Important

The PRESTO! pressure interpolation scheme, when used with the non-iterative time-advance-

ment solver, is less stable than in the case of the iterative time-advancement solver. As a con-

sequence, smaller time steps may be required.

As mentioned above, the default control settings are optimally designed to obtain a second-

order solution. In order to save CPU time, in cases where transient accuracy is not a main concern

(that is, first-order integration in time and space), or when NITA is used to converge toward a

steady-state solution, you may want to set the Max. Corrections value to  in the Advanced

Solution Controls dialog box (Expert tab) for all transport equations except pressure.

For transient simulations that use the pressure-based solver, the order in which the model equations

are solved can affect the speed of convergence. You can specify the equation order using the following

solve → set → equation-ordering

Note that the standard method is enabled by default and corresponds to the ordering shown in

Figure . : Overview of the Iterative Time Advancement Solution Method For the Segregate Solver

and Figure . : Overview of the Non-Iterative Time Advancement Solution Method in the Theory

Guide; alternatively, you can select the optimized-for-volumetric-expansion method, which

is recommended for flows in which the density is strongly dependent on thermal effects, chemical

composition, and so on (such as combustion simulations). This text command is not available when a

multiphase model is enabled.

To use the density-based solver you must first select the solver type, and determine if the simulation

is steady-state or transient from the General Task Page (see Choosing the Solver (p. )). The density

based solver settings are available mainly in two task pages: the Solution Methods Task Page (p. )

and the Solution Controls Task Page (p. ).

In the Solution Methods task page, you can select the following:

Solution formulation type: Implicit or Explicit

Flux Scheme type : Roe-FDS, AUSM, or Low Diffusion Roe-FDS

Flow equation and model equation spatial discretization accuracy

For the steady-state solution method, you can select additional solution options to accelerate conver-

gence

– Pseudo transient solution method

– Convergence acceleration for stretched meshes

For the transient formulation you can select

– first-order implicit

– second-order implicit and for the explicit solver formulation, you can also select the explicit transient

formulation

In the Solution Controls task page, you can select the following:

For the density-based explicit solver, you will specify the Courant number, FAS multigrid level, and

Residual smoothing

For the density-based implicit solver, you will need to enter only the Courant number

For both solver methods, you will enter the under-relaxation factors associated with other equations

solved with the flow equations, such as equations of the turbulence model

The above options can be found in the following sections:

... Changing the Courant Number

... Convective Flux Types

... Convergence Acceleration for Stretched Meshes (CASM)

... Preventing Divergence Using Local Under-Relaxation

... Specifying the Explicit Relaxation

...Turning On FAS Multigrid

For ANSYS Fluent’s density-based solver, the main control over the time-stepping scheme is the

Courant number (CFL). The time step is proportional to the CFL, as defined in Equation . in the

Density-Based Solver Settings

Linear stability theory determines a range of permissible values for the CFL (that is, the range of values

for which a given numerical scheme will remain stable). When you specify a permissible CFL value,

ANSYS Fluent will compute an appropriate time step using Equation . in the Theory Guide. In

general, taking larger time steps leads to faster convergence, so it is advantageous to set the CFL as

large as possible (within the permissible range).

The stability limits of the density-based implicit and explicit formulations are significantly different.

The explicit formulation has a more limited range and requires lower CFL settings than does the

density-based implicit formulation. Appropriate choices of CFL for the two formulations are discussed

below.

.... Courant Numbers for the Density-Based Explicit Formulation

Linear stability analysis shows that the maximum allowable CFL for the multi-stage scheme used in

the density-based explicit formulation will depend on the number of stages used and how often the

dissipation and viscous terms are updated (see Changing the Multi-Stage Scheme (p. )). But in

general, you can assume that the multi-stage scheme is stable for Courant numbers up to .. This

stability limit is often lower in practice because of nonlinearities in the governing equations.

The default CFL for the density-based explicit formulation is ., but you may be able to increase it

for some 2D problems. You should generally not use a value higher than ..

If your solution is diverging, that is, if residuals are rising very rapidly, and your problem is properly

set up and initialized, this is usually a good sign that the Courant number must be lowered. Depending

on the severity of the startup conditions, you may need to decrease the CFL to a value as low as .

to . to get started. Once the startup transients are reduced you can start increasing the Courant

number again.

.... Courant Numbers for the Density-Based Implicit Formulation

Linear stability theory shows that the density-based implicit formulation is unconditionally stable.

However, as with the explicit formulation, nonlinearities in the governing equations will often limit

stability.

The default CFL for the density-based implicit formulation is .. It is often possible to increase the

CFL to , , , or even higher, depending on the complexity of your problem. You may find that

a lower CFL is required during startup (when changes in the solution are highly nonlinear), but it can

be increased as the solution progresses.

The coupled AMG solver has the capability to detect divergence of the multigrid cycles within a given

iteration. If this happens, it will automatically reduce the CFL and perform the iteration again, and a

message will be printed to the screen. Five attempts are made to complete the iteration successfully.

Upon successful completion of the current iteration the CFL is returned to its original value and the

iteration procedure proceeds as required.

The Courant number is set in the Solution Controls Task Page (p. ) (Figure . : The Solution Controls

Task Page for the Density-Based Explicit Formulation (p. )).

Solution →

Controls

Figure . : The Solution Controls Task Page for the Density-Based Explicit Formulation

Enter the value for Courant Number.

When you select Explicit from the Formulation drop-down list in the Solution Methods Task

Page (p. ), ANSYS Fluent will automatically set the Courant Number to ; when you select Implicit

from the Formulation drop-down list, the Courant Number will be changed to  automatically.

The convective fluxes are selected from the Flux Type drop-down list in the Solution Methods task

page.

Solution →

Methods

You can select from the following when using the density-based solver:

Roe flux-difference splitting (Roe-FDS)

Roe-FDS splits the fluxes in a manner that is consistent with their corresponding flux method eigen-

values. It is the default and is recommended for most cases.

Advection Upstream Splitting Method (AUSM)

AUSM provides exact resolution of contact and shock discontinuities and it is less susceptible to

Carbuncle phenomena.

Low diffusion Roe flux-difference splitting (Low Diffusion Roe-FDS)

Low Diffusion Roe-FDS is available when a Scale-Resolving Simulation (SRS) turbulence model is

enabled along with the time-implicit formulation. It reduces the dissipation in turbulence calculations.

This should be used only for subsonic flows.

Note

For cases that use an SRS turbulence model and/or include acoustic calculations, it is recom-

mended that you use the Roe-FDS with the Bounded Central Differencing (BCD) discret-

ization scheme selected for the flow equations, as this combination is more numerically

robust than Low Diffusion Roe-FDS and just as accurate. The BCD scheme alters the

standard Roe-FDS scheme such that the diffusion is reduced. Note that if you are not using

an SRS turbulence model, to access the BCD scheme you will first need to type the

solve/set/expert text command and enter yes when asked if you want to Allow

selection of all applicable discretization schemes?.

When using the density-based solver with the implicit solution formulation in steady-state you can

accelerate the convergence of your solution on highly-stretched and anisotropic meshes (like the one

used when modeling external aerodynamic problems) by selecting the Convergence Acceleration

For Stretched Meshes in the Solution Methods task page. For further information and theoretical

background on this solution acceleration option, see Convergence Acceleration for Stretched Meshes

in the Theory Guide. The Convergence Acceleration For Stretched Meshes option provides an op-

timum solution convergence of the implicit solution method.

To apply convergence acceleration for stretched meshes, perform the following:

. Specify the solver options by selecting Density-Based and Steady in the General task page.

. Select Implicit from the Formulation drop-down list and enable Convergence Acceleration For

Stretched Meshes in the Solution Methods task page (Figure . :The Solution Methods Task Page

for the Density-Based Implicit Formulation (p. )).

Figure . : The Solution Methods Task Page for the Density-Based Implicit Formulation

Extra settings for CASM can be set using the following text command:

solve → set → convergence-acceleration-for-stretched-meshes/

Enter yes in response to the Use convergence acceleration for stretched meshes

(CASM)? question. You will also be asked for a cut-off on the CFL value multiplier. By default this

value is set to . Typically, you do not need to adjust this value. But if convergence difficulties are

encountered and reduction of the CFL value alone does not help improve convergence, then it is ad-

visable to reduce this CFL multiplier cut-off to a lower value (for example from  to ,  or ).

The use of CASM can typically give a much faster convergence over the standard solution method. In

general, when using CASM, you do not need to specify a very large CFL value as you do with the

standard solution method. A CFL value between  and  is typically used for converging most flow

problems. When the Convergence Acceleration For Stretched Meshes option is selected, the solver

will run when appropriate with a variable local CFL value proportional to the cell aspect ratios. Therefore,

when the cell aspect ratio nears unity (typically far from walls), the local cell CFL value will be the same

as the value that you supplied. However, as the cell is stretched and the cell aspect ratio increases

(near walls), the local cell CFL value will be multiplied by the cell aspect ratio value. This is true until

the cell stretching is beyond the multiplier cut-off value specified using the text command. The pro-

portional change in CFL value on highly stretched cells helps accelerate the solution especially on

highly packed and stretched meshes like the one used in modeling external flow problems.

When the cell aspect ratio is selected by default, the density based implicit solver will operate with an

explicit relaxation of . which can be adjusted from the Explicit underrelaxation value

entry in solve → set → expert

The convergence of the solution is mainly controlled by adjusting the CFL value. Therefore, if conver-

gence problems are encountered, lowering the CFL value will help improve the convergence. Additional

solution parameters to be adjusted for more conservative solution settings are:

. lowering the density-based implicit solver explicit relaxation (solve → set → expert)

. adjusting the CFL multiplier cut-off value to a lower value (solve → set → convergence-accel-

eration-for-stretched-meshes/)

This solution convergence method is very aggressive. Therefore it is of paramount importance to start

with a good initial guess especially if you start with second order spatial discretization. To get a good

starting solution with the guess you provide, you are advised to use the full multi-grid initialization

method (see Full Multigrid (FMG) Initialization (p. )).

Note

When selecting the Convergence Acceleration For Stretched Meshes option then the

Pseudo-Transient solution method will not be available. You can either use Convergence

Acceleration For Stretched Meshes or the Pseudo-Transient solution method. These two

options cannot be used at the same time. Both methods help in obtaining faster convergence

on anisotropic meshes. But one method requires that you enter a CFL value, while the

other requires that you enter a pseudo-time step value to march the solution to convergence.

It is up to you to select the method with which you are most comfortable.

Convergence Acceleration For Stretched Meshes shows an advantage over the standard

solution method, particularly with stretched meshes with low Y+ values (near unity). The

use of Convergence Acceleration For Stretched Meshes results in an alteration of the

numerical dissipation of the selected flux scheme. This change may slightly impact the

monitored loading level if compared with the solution obtained without the use of this

option.

It is a sign of local divergence when the temperature and/or pressure for individual cells approaches

the minimum and/or maximum limits (set in the Solution Limits Dialog Box (p. )), and this can precede

the divergence of the global solution. If either of these quantities is being reset to a limiting value re-

peatedly (as indicated by the appropriate warning messages in the console), you should check the

dimensions, boundary conditions, and properties to be sure that the problem is set up correctly, and

try to determine the cause; you can create a field variable cell register to mark and display cells have

a value equal to the limit (refer to Field Variable (p. ) for more information). If the setup appears

appropriate but the density-based solver still diverges, it is recommended that you use divergence

prevention, which has been shown to be helpful for challenging cases (such as those that undergo

shocks or experience difficulties related to species calculations). With this option, Fluent will identify

the locally diverging cells and automatically apply a treatment to them that freezes the pressure and/or

temperature values (that is, sets the under-relaxation factor—which is similar to  in Equation .

in the Fluent Theory Guide—to ) and applies under-relaxation to the other variables. To enable diver-

gence prevention, use the following text command:

solve → set → divergence-prevention → enable?

When prompted, enter yes, and then define the under-relaxation factor for the other variables: the

default value of . is recommended, though if this fails to prevent divergence you can try increasing

this under-relaxation by reducing the factor to .

Note

When you decide to enable divergence prevention, note the following: if the warning

messages indicate that only a small percentage of cells are approaching the temperature

and/or pressure limits, then you can just continue the calculation; if the percentage of cells

is a higher value, it is recommended that you restart the calculation from initialization.

To improve the convergence to steady-state for some flow cases when using the density-based implicit

solver you can specify the explicit relaxation using the following text command:

Enter a value between  and  in response to the Explicit relaxation value prompt.

For more information about explicit relaxation, see Under-Relaxation of Variables in the Theory Guide.

As discussed in Multigrid Method in the Theory Guide, FAS multigrid is an optional component of the

density-based explicit formulation, while AMG multigrid is always on, by default for the density-based

implicit formulation. Since nearly all density-based explicit calculations will benefit from the use of the

FAS multigrid convergence accelerator, you should generally set a nonzero number of coarse grid

levels before beginning the calculation. For most problems, this will be the only FAS multigrid para-

meter you will need to set. Should you encounter convergence difficulties, consider applying one of

the methods discussed in Setting FAS Multigrid Parameters (p. ).

Important

Note that you cannot use FAS multigrid with explicit time stepping (described in Temporal

Discretization in the Theory Guide) because the coarse grid corrections will destroy the time

accuracy of the fine grid solution.

.... Setting Coarse Grid Levels

As discussed in Full-Approximation Storage (FAS) Multigrid in the Theory Guide, FAS multigrid solves

on successively coarser grids and then transfers corrections to the solution back up to the original

fine grid, thereby increasing the propagation speed of the solution and speeding convergence. The

most basic way you can control the multigrid solver is by specifying the number of coarse grid levels

to be used.

As explained in Full-Approximation Storage (FAS) Multigrid in the Theory Guide, the coarse grid levels

are formed by agglomerating a group of adjacent “fine” cells into a single “coarse” cell. The optimal

number of grid levels is therefore problem-dependent. For most problems, you can start out with

or  levels. For large 3D problems, you may want to add more levels (although memory restrictions

may prevent you from using more levels, since each coarse grid level requires additional memory).

If you believe that multigrid is causing convergence trouble, you can decrease the number of levels.

If ANSYS Fluent reaches a coarse grid with one cell before creating as many levels as you requested,

it will simply stop there. That is, if you request  levels, and level  has only  cell, ANSYS Fluent will

create only  levels, since levels  and  would be the same.

To specify the number of grid levels you want, set the number of Multigrid Levels in the Solution

Controls Task Page (p. ) (Figure . : The Solution Controls Task Page for the Density-Based Explicit

Formulation (p. )).

Solution →

Controls

You can also set the Max Coarse Levels under FAS Multigrid Controls in the Multigrid tab in the

Advanced Solution Controls Dialog Box (p. ).

Changing the number of coarse grid levels in the Solution Controls task page will automatically

update the number shown in the Multigrid tab in the Advanced Solution Controls Dialog Box (p. ).

Coarse grid levels are created when you first begin iterating. If you want to check how many cells

are in each level, request one iteration and then click Info and select Size in the Domain ribbon tab

(Mesh group box) (as described in Mesh Size (p. )) to list the size of each grid level. If you are sat-

isfied, you can continue the calculation; if not, you can change the number of coarse grid levels and

check again.

For most problems, you will not need to modify any additional multigrid parameters once you have

settled on an appropriate number of coarse grid levels. You can simply continue your calculation

until convergence.

.... Using Residual Smoothing to Increase the Courant Number

In the density-based explicit formulation, implicit residual smoothing (or averaging) is a technique

that can be used to reduce the time step restriction of the solver, thereby allowing the Courant

number to be increased. The implicit smoothing is implemented with an iterative Jacobi method, as

described in Implicit Residual Smoothing in the Theory Guide. Solution Controls Task Page (p. ).

Solution →

Controls

By default, the number of Iterations for Residual Smoothing is set to zero, indicating that residual

smoothing is disabled. If you increase the Iterations counter to  or more, you can enter the

Smoothing Factor. A smoothing factor of . with  passes of the Jacobi smoother is usually adequate

to allow the Courant number to be doubled.

As mentioned earlier, in most cases the multigrid solver will not require any special attention from you.

If, however, you have convergence difficulties or you want to minimize the overall solution time by

using more aggressive settings, you can monitor the multigrid solver and modify the parameters to

improve its performance. (The instructions below assume that you have already begun calculations,

since there is no need to monitor the solver if you do not fit into one of the two categories above.)

To determine whether your convergence difficulties can be alleviated by modifying the multigrid settings,

you will check if the requested residual reduction is obtained on each grid level. To minimize solution

time, you will check to see if switching to a more powerful cycle will result in overall reduction of work

by the solver.

By default, the flexible cycle is used for all equations except pressure correction, which uses a V cycle.

Typically, for a flexible cycle only a few (–) relaxations will be performed at the finest level and no

coarse levels will be visited. In some cases one or two coarse levels may be visited. If the maximum

number of fine level relaxations is not sufficient, you may want to increase the maximum number (as

described in Flexible Cycle Parameters (p. )) or switch to a V cycle (as described in Specifying the

Multigrid Cycle Type (p. )).

In the pressure-based segregated algorithm, the pressure correction uses a V cycle by default. If the

maximum number of cycles ( by default) is not sufficient, you can switch to a W cycle (using the

Multigrid tab in the Advanced Solution Controls Dialog Box (p. ), as described in Specifying the

Multigrid Cycle Type (p. )). Note that efficiency may deteriorate with a W cycle.

You can try increasing the maximum number of cycles by increasing the value of Max Cycles in the

Multigrid tab, under Fixed Cycle Parameters.

In the pressure-based coupled algorithm and the density-based implicit formulation, there is no pressure

correction. Instead, there is a flow correction, which by default uses the F cycle. The density-based ex-

plicit formulation uses the V cycle as the default flow correction.

Solution →

Setting Algebraic Multigrid Parameters

Figure . : The Multigrid Tab

... Specifying the Multigrid Cycle Type

... Setting the Termination and Residual Reduction Parameters

... Setting the Stabilization Method

... Additional Algebraic Multigrid Parameters

... Setting FAS Multigrid Parameters

By default, the V cycle is used for the pressure equation in the pressure-based segregated algorithm

and the flexible cycle is used for all other equations with the exception that the F cycle is used for

energy. In the pressure-based coupled algorithm, the F cycle is the default for the coupled flow

equations and for the energy equation. All other scalar equations use the flexible cycle by default. In

the density-based implicit formulation, the F cycle is default for the flow correction. The V cycle is default

for the flow correction in the density-based explicit formulation. For both density-based formulations

the flexible cycle is used for the scalar equations. (See Multigrid Cycles in the Theory Guide for a de-

scription of these cycles.) To change the cycle type for an equation, you will use the top portion of

the Multigrid tab in the Advanced Solution Controls Dialog Box (p. ) (Figure . : The Multigrid

Tab (p. )).

For each equation, you can choose Flexible, V-Cycle, W-Cycle, or F-Cycle in the adjacent drop-down

list.

When you use the flexible cycle for an equation, you can control the multigrid performance by modi-

fying the Termination and/or Restriction criteria for that equation at the top of the Multigrid tab in

the Advanced Solution Controls Dialog Box (p. ) (Figure . : The Multigrid Tab (p. )).

Solution →

The Restriction criterion is the residual reduction tolerance,

This parameter dictates when a coarser grid level must be visited (due to insufficient improvement in

the solution on the current level). With a larger value of , coarse levels will be visited less often (and

vice versa). The Termination criterion,

in Equation . in the Theory Guide, governs when the

solver should return to a finer grid level (that is, when the residuals have improved sufficiently on the

current level).

For the V, W, or F cycle, the Termination criterion determines whether or not another cycle should

be performed on the finest (original) level. If the current residual on the finest level does not satisfy

Equation . in the Theory Guide, and the maximum number of cycles has not been performed,

ANSYS Fluent will perform another multigrid cycle. (The Restriction parameter is not used by the V,

W, and F cycles.)

The AMG solver  [] (p. ) builds coarse levels by grouping fine level cells to make coarse level

cells, and uses piecewise constant interpolation.

In the Multigrid tab (Figure . : The Multigrid Tab (p. )), you can choose another stabilization

method rather than the AMG solver if you are using a fixed-type cycle (F, V, or W cycle); this is available

for all equations except the flow correction for the density-based solver. If desired, you can choose

the bi-conjugate gradient stabilized method  [] (p. ) (BCGSTAB) option, the recursive projection

method  [] (p. ) (RPM), or the generalized minimal residual method [] (p. ) (GMRES) in

order to improve the convergence of the linear solver. BCGSTAB and GMRES can be preconditioned,

and all these methods can provide more stability and robustness than the AMG solver.

ANSYS Fluent usually builds diagonally dominant matrices for the linear solver. However, this is not

always possible. A linear system with highly dominant off-diagonal coefficients may occur during dis-

cretization of complex physical models such as multiphase cavitation. Using a stabilization method in

such cases can be helpful. In addition, the AMG convergence in parallel can be improved using the

BCGSTAB or GMRES option with AMG. It is recommended that you attempt a solution first with

BCGSTAB; the GMRES is usually more robust and more likely to converge, but it is more demanding

in terms of memory usage and solver time.

If you are using the pressure-based segregated solver and the flow is incompressible, an additional

stabilization method for the algebraic multigrid solver will appear in the Stabilization Method drop-

down list. This is the conjugate gradient method, or CG [] (p. ) and will be available only for the

pressure equation. This method is typically used in conjunction with an AMG preconditioner (any

available AMG method). The CG formulation requires a symmetric system matrix. Such matrices result

from the finite volume discretization of steady or transient elliptic operators, such as the pressure

correction equation in the incompressible case. The CG method provides a useful alternative to BCGSTAB,

RPM, and GMRES, since it reduces the memory requirements and the number of floating point opera-

tions, especially when compared to BCGSTAB. In addition, in transient pressure-based segregated

solvers, as typically used in LES and/or NITA simulations, the solution of the pressure correction

equation constitutes a significant share of the overall computational effort.

Note that when divergence is detected for the AMG solver, the BCGSTAB method and/or the CG

method, then an alternate method will be used for an iteration as a fallback, and you will be informed

in the console that an equation is being stabilized to enhance linear solver robustness. If you see such

console messages repeatedly for flow-related equations, it is an indication that you need to revise the

settings in the Solution Methods task page and/or the Algebraic Multigrid Controls group box of

the Advanced Solution Controls dialog box.

There are several additional parameters that control the algebraic multigrid solver, but there will usually

be no need to modify them. These additional scalar and coupled parameters are all contained in the

Multigrid tab in the Advanced Solution Controls Dialog Box (p. ) (Figure . : The Multigrid

Tab (p. )).

Solution →

Important

When using the density-based explicit formulation or the pressure-based solver with any

of the segregated algorithms, described in Pressure-Velocity Coupling in the Theory Guide

and Choosing the Pressure-Velocity Coupling Method (p. ), only Scalar Parameters are

set in the Multigrid tab. If you use the density-based implicit or the pressure-based coupled

algorithm, described in Coupled Algorithm in the Theory Guide, then you can set the

Coupled Parameters.

.... Fixed Cycle Parameters

For the fixed (V, W, and F) multigrid cycles, you can control the number of pre- and post-relaxations

(

and

in Multigrid Cycles in the Theory Guide). Pre-Sweeps sets the number of relaxations to

perform before moving to a coarser level. Post-Sweeps sets the number to be performed after

coarser level corrections have been applied. Normally, under Scalar Parameters, one post-relaxation

is performed and no pre-relaxations are done (that is,

and

), but in rare cases, you may

need to increase the value of

and

to  or . Under Coupled Parameters, three post-relaxations are

performed by default with no pre-relaxations. If you are using the pressure-based coupled solver for

a steady simulation with pseudo-transient enabled, three post-relaxations are performed under

Scalar Parameters also.

Important

If you are using AMG with V-cycle to solve an energy equation with a solid conduction model

presented with anisotropic or very high conductivity coefficient, there is a possibility of diver-

gence with a default post-relaxation sweep of . In such cases you should increase the post-

relaxation sweep (to say ) in the AMG section for better convergence when using the pressure-

based segregated algorithms.

It is recommended that you use the Fixed F-cycle for the energy equation when running parallel

.... Coarsening Parameters

For all multigrid cycle types, you can control the maximum number of coarse levels (Max Coarse

Levels under Scalar or Coupled Parameters) that will be built by the multigrid solver.

Sets of coarser simultaneous equations are built until the maximum number of levels has been created,

or the coarsest level has only  equations. Each level has about half as many unknowns as the previous

level, so coarsening until there are only a few cells left will require about as much total coarse-level

coefficient storage as was required on the fine mesh. Reducing the maximum coarse levels will reduce

the memory requirements, but may require more iterations to achieve a converged solution. Setting

Max Coarse Levels to  turns off the algebraic multigrid solver.

Another coarsening parameter you can control is the increase in coarseness on successive levels. The

Coarsen by parameter specifies the number of fine grid cells that will be grouped together to create

a coarse grid cell. The algorithm groups each cell with its strongest neighbor, then groups the cell

and its strongest neighbor with the neighbor’s strongest neighbor, continuing until the desired

coarsening is achieved. Typical values for the scalar parameters are in the range from  to , with

the default value of  for the Gauss-Seidel smoother giving the best performance, but also the greatest

memory use. For coupled parameters and scalar parameters when using the pressure-based coupled

solver with pseudo-transient enabled, the default values of  (for 2D) and  (for 3D) for the ILU

smoother give the best performance. You should not adjust this parameter unless you need to reduce

the memory required to run a problem.

Important

Depending on the smoother type, Gauss-Seidel or ILU, the Coarsen by and Post-Sweeps

settings should be changed as follows when selecting the non-default smoother type:

ILU

: Post-Sweeps= and Coarsen by =

Gauss-Seidel

For the scalar and coupled equations, you have the following AMG coarsening options. Note that

these can be used singly or in combination with each other.

Conservative Coarsening

This option is enabled by default, and improves convergence for difficult problems by tuning

multigrid coarsening based on coefficient strengths and, in parallel computations, the partitioning.

Aggressive Coarsening

This option specifies the use of a version of the AMG solver that is optimized for higher, more ag-

gressive coarsening rates. It is recommended if the AMG solver diverges with the default settings,

and is more likely to be beneficial in the following cases:

– if the corresponding Coarsen by field is set to a value greater than  (which is the case by default if

you are using the density-based implicit or the pressure-based coupled scheme)

– if you are using higher core counts

Laplace Coarsening

This option is disabled by default, so that a cell’s strongest neighbor is identified based on the

magnitude of its interaction with the cell in question. Enabling it specifies that Laplace coefficients

are used to evaluate neighbor strength when grouping cells for coarsening. This may improve

stability in some cases because the coarser levels will not change as the solution evolves. It may

also reduce computation time, particularly at high core counts, because the coarse levels don’t

need to be recreated every iteration.

.... Smoother Types

Two smoother types are available for scalar and coupled parameters. Gauss-Seidel is the simplest

smoother type and is recommended when using the pressure-based segregated algorithm. ILU is

more CPU intensive, but has better smoothing properties for block-coupled systems such as the

pressure-based coupled solver and the density-based implicit formulation. The default scalar

Smoother Type is Gauss-Seidel, while the coupled Smoother Type is ILU. The ILU smoother is also

used for scalar equations when using the coupled solver with pseudo-transient enabled. For more

information about the two smoother types, see The Coupled and Scalar AMG Solvers in the Theory

Guide.

.... Flexible Cycle Parameters

To change the maximum number of relaxations, increase or decrease the value of Max Fine Relaxa-

tions or Max Coarse Relaxations in the Multigrid tab in the Advanced Solution Controls Dialog

Box (p. ) (Figure . : The Multigrid Tab (p. )) under Flexible Cycle Parameters.

Solution →

.... Setting the Verbosity

The steps for monitoring the solver are as follows:

. Set multigrid Verbosity to  or  in the Multigrid tab in the Advanced Solution Controls Dialog Box (p. ).

Solution →

. Request a single iteration using the Run Calculation Task Page (p. ).

Solution →

If you set the verbosity to , the information printed in the ANSYS Fluent console for each equation

will include the following:

equation name

equation tolerance (computed by the solver using a normalization of the source vector)

residual value after each fixed multigrid cycle or fine relaxation for the flexible cycle

number of equations in each multigrid level, with the zeroth level being the original (finest-level) system

of equations

Note that the residual printed at cycle or relaxation  is the initial residual before any multigrid cycles

are performed.

When verbosity is set to , only the equation name, tolerance, and residuals are printed.

A portion of a sample printout is shown below:

pressure correction equation:

tol. .2668e-

.5336e+

.9778e-

.5863e-

.9387e-

multigrid levels:

.... Returning to the Default Multigrid Parameters

If you change the multigrid parameters, but you then want to return to ANSYS Fluent’s default settings,

you can click the Default button in the Multigrid tab. ANSYS Fluent will change all settings to the

defaults, and the Default button will become the Reset button. To get your settings back again, you

can click the Reset button.

For most calculations, you will not need to modify any FAS multigrid parameters once you have set

the number of coarse grid levels. If, however, you encounter convergence difficulties, you may consider

the following suggested procedures.

Important

Recall that FAS multigrid is used only by the density-based explicit formulation.

.... Combating Convergence Trouble

Some problems may approach convergence steadily at first, but then the residuals will level off and

the solution will “get stuck.” In some cases (for example, long thin ducts), this convergence trouble

may be due to multigrid’s slow propagation of pressure information through the domain. In such

cases, you should turn off multigrid by setting Multigrid Levels to  in the Solution Controls Task

Page (p. ).

....“Industrial-Strength” FAS Multigrid

In some cases, you may find that your problem is converging, but at an extremely slow rate. Such

problems can often benefit from a more aggressive form of multigrid, which will speed up the

propagation of the solution corrections. For such problems, you can try the “industrial-strength”

multigrid settings.

Important

These settings are very aggressive and assume that the solution information passed through

the multigrid levels is somewhat accurate. For this reason, you should only attempt the

procedure described here after you have performed enough iterations that the solution is

off to a good start. Using “industrial-strength” multigrid too early in the calculation pro-

cess—when the solution is far from correct—will not help convergence and may cause

the calculation to become unstable, as very incorrect values are propagated quickly to the

original grid. Note also that while these multigrid settings will usually reduce the total

number of iterations required to reach convergence, they will greatly increase the compu-

tation time for each multigrid cycle. Thus the solver will be performing fewer but longer

iterations.

The strategy employed is as follows:

Increase the number of iterations performed on each grid level before proceeding to a coarser level

Increase the number of iterations performed on each grid level after returning from a coarser level

Allow full correction transfer from one level to the next finer level, instead of transferring reduced values

of the corrections

Do not smooth the interpolated corrections when they are transferred from a coarser grid to a finer grid

You can set all of the parameters for this strategy under FAS Multigrid Controls in the Multigrid

tab in the Advanced Solution Controls Dialog Box (p. ) (Figure . : The Advanced Solution Controls

Dialog Box (p. )) and then continue the calculation.

Solution →

Figure . : The Advanced Solution Controls Dialog Box

Increasing the number of iterations performed on each grid level before proceeding to a coarser level

(the value of

described in Multigrid Cycles in the Theory Guide) will improve the solution passed

from each finer grid level to the next coarser grid level. Try increasing the value of Pre-Sweeps (under

FAS Multigrid Controls, not under Algebraic Multigrid Controls) to .

Increasing the number of iterations performed on each level after returning from a coarser level will

improve the corrections passed from each coarser grid level to the next finer grid level. Errors intro-

duced on the coarser grid levels can therefore be reduced before they are passed further up the grid

hierarchy to the original grid. Try increasing the value of Post-Sweeps (under FAS Multigrid Controls,

not under Algebraic Multigrid Controls) to .

By default, the full values of the multigrid corrections are not transferred from a coarser grid to a

finer grid; only % of the value is transferred. This prevents large errors from transferring quickly up

to the original grid and causing the calculation to become unstable. It also prevents a “good” solution

from propagating quickly to the original grid. However, by increasing the Correction Reduction to

, you can transfer the full values from coarser to finer grid levels, speeding the propagation of the

solution and, usually, the convergence as well. The Species Correction Reduction sets the factor by

which to reduce the magnitude of the species corrections to stabilize the multigrid calculation. This

item appears only when species transport is being modeled.

When the corrections on a coarse grid are passed back to the next finer grid level, the values are, by

default, interpolated and then smoothed. Disabling the smoothing so that the actual value in a coarse

grid cell is assigned to the fine grid cells that make it up can also aid convergence. To disable

smoothing, set the Correction Smoothing to . Large discontinuities between cells will be smoothed

out implicitly as a result of the additional Post-Sweeps performed.

The Courant Number Reduction sets the factor by which to reduce the Courant number for coarse

grid levels (that is, every level except the finest). Some reduction of time step (such as the default

.) is typically required because the stability limit cannot be determined as precisely on the irregularly

shaped coarser grid cells.

In order to keep the solution stable under extreme conditions, ANSYS Fluent provides limits that keep

the solution within an acceptable range. You can control these limits with the Solution Limits Dialog

Box (p. ) (Figure . : The Solution Limits Dialog Box (p. )).

Limits...

Figure . : The Solution Limits Dialog Box

Setting Solution Limits

Fluent applies limiting values for pressure, static temperature, and turbulence quantities. Fluent also

applies a minimum volume fraction for the matrix solution in Eulerian multiphase simulations run on

a double-precision solver. The purpose of these limits is to keep the absolute pressure or static temper-

ature from becoming zero, negative, or excessively large during the calculation, and to keep the turbu-

lence quantities from becoming excessive. The purpose of the minimum volume fraction is to avoid

singularity of the solution matrix when the volume fraction tends to zero.

Typically, you will not need to change the default solution limits. If pressure, temperature, or turbulence

quantities are being reset to the limiting value repeatedly (as indicated by the appropriate warning

messages in the console), you should check the dimensions, boundary conditions, and properties to be

sure that the problem is set up correctly and try to determine why the variable in question is getting

so close to zero or so large. You can create a field variable cell register to mark and display cells have

a value equal to the limit (refer to Field Variable (p. ) for more information). In very rare cases, you

may need to change the solution limits, but only do so if you are sure that you understand the reason

for the solver’s unusual behavior. For example, you may know that the temperature in your domain

will exceed  K. Be sure that any temperature-dependent properties are appropriately defined for

high temperatures if you increase the maximum temperature limit. Another rare example is when the

actual volume fraction in the domain needs to go below a safe limit of 1e-, such as in nucleation and

dispersion of very low amounts of contaminants in a system. By reducing this limit you may encounter

instability problems.

Important

Important

The absolute pressure limit is enforced only for fluid materials that are modeled using the

ideal-gas or one of the real-gas-* density methods.

For materials that use the compressible-liquid or a user-defined compressible fluid (liquid or

gas) density method, a pressure limit is used to ensure that the density remains positive, but

the actual pressure value itself is not limited.

Note that if you are using the density-based solver and the temperature and/or pressure values are

approaching the minimum and/or maximum limits, you can enable divergence prevention to apply

under-relaxation to the variables in select cells rather than changing the limits. For details, see Preventing

Divergence Using Local Under-Relaxation (p. ).

... Limiting the Values of Solution Variables

... Adjusting the Positivity Rate Limit

... Resetting Solution Limits

The limiting minimum and maximum values for absolute pressure are shown in the Minimum and

Maximum Absolute Pressure fields. If the ANSYS Fluent calculation predicts a value less than the

Minimum Absolute Pressure or greater than the Maximum Absolute Pressure, the corresponding

limiting value will be used instead. Similarly, the Minimum and Maximum Temperature are limiting

values for energy calculations.

The Minimum Turb. Kinetic Energy, Minimum Turb. Dissipation Rate, and the Maximum Turb.

Viscosity Ratio are limiting values for turbulent calculations. If the calculation predicts a value for

or  that is less than the appropriate limiting value (that is, Minimum Turb. Kinetic Energy or Minimum

Turb. Dissipation Rate, respectively), then the limiting value will be used instead. For the viscosity

ratio limit, ANSYS Fluent uses the limiting maximum value of turbulent viscosity (

) in the flow

field relative to the laminar viscosity. If the ratio calculated by ANSYS Fluent exceeds the limiting value,

the ratio is set to the limiting value by limiting  to the necessary value.

For Eulerian and Mixture multiphase simulations run on a double-precision solver using the implicit

volume fraction formulation, if the prediction of volume fraction falls below the value specified for

Minimum Vol. Frac. for Matrix Solution, ANSYS Fluent will use the limiting value in the matrix solution

for phase-specific equations, depending on the model.

For the multiphase models supporting the explicit volume fraction formulation and for the VOF model,

the Volume Fraction Cutoff limit specified in the Multiphase Model dialog box will serve as a limiting

value when solving phase-specific equations, depending on the model.

Note

The Eulerian multiphase model uses the specified solution limits for solving Momentum,

Turbulence, Energy, Species, and UDS equations, whereas the VOF and Mixture multiphase

models use the specified limits for solving Species and UDS equations.

In ANSYS Fluent’s density-based solver, the rate of reduction of temperature is controlled by the Pos-

itivity Rate Limit. The default value of ., for example, means that temperature is not allowed to

decrease by more than % of its previous value from one iteration to the next. If the temperature

change exceeds this limit, the time step in that cell is reduced to bring the change back into range

and a “time step reduced” warning is printed. (This reduced time step will be used for the solution of

all variables in the cell, not just for temperature.) Rapid reduction of temperature is an indication that

the temperature may become negative. Repeated “time step reduced” warnings should alert you that

something is wrong in your problem setup. (If the warning messages stop appearing, the calculation

may have “recovered” from the time-step reduction.)

Important

For high-speed flow, if your solution is diverging particularly for the energy equation, then

lowering this limit to . or . might help in overcoming divergence.

If you change and save the value of one of the solution limits, but you then want to return to the default

limits set by ANSYS Fluent, you can reopen the Solution Limits Dialog Box (p. ) and click the Default

button. ANSYS Fluent will change the values to the defaults and the Default button will become the

Reset button. To get your values back again, you can click the Reset button.

The most common parameter you will change to control the convergence of the multi-stage time-

stepping scheme is the Courant number. Instructions for modifying the Courant number are presented

in Changing the Courant Number (p. ). The Multi-Stage tab is accessible from the Advanced Solution

Controls dialog box when using the density-based explicit formulation.

Setting Multi-Stage Time-Stepping Parameters

... Changing the Multi-Stage Scheme

It is possible to make several changes to the multi-stage time-stepping scheme itself. You can change

the number of stages and set a new multi-stage coefficient for each stage. You can also control

whether or not dissipation and viscous stresses are updated at each stage. These changes are made

in the Multi-Stage tab in the Advanced Solution Controls Dialog Box (p. ) (Figure . : The Multi-

Stage Tab (p. )).

Figure . : The Multi-Stage Tab

Important

You should not attempt to make changes to ANSYS Fluent’s multi-stage scheme unless you

are very familiar with multi-stage schemes and are interested in trying a different scheme

found in the literature.

.... Changing the Coefficients and Number of Stages

By default, the ANSYS Fluent multi-stage scheme uses  stages for steady-state solutions with coeffi-

cients of ., ., and ., and  stages for unsteady solutions with coefficients of ., .,

., and .. You can decrease or increase the number of stages using the arrow buttons for Number

of Stages in the Multi-Stage tab. (If you want to increase the number of stages beyond five, you will

need to use the text-interface command solve/set/multi-stage.)

For each stage, you can modify the Coefficient. Coefficients must be greater than  and less than .

The final stage should always have a coefficient of .

.... Controlling Updates to Dissipation and Viscous Stresses

For each stage, you can indicate whether or not artificial dissipation and viscous stresses are evaluated.

If a Dissipation box is selected for a particular stage, artificial dissipation will be updated on that

stage. If not selected, artificial dissipation will remain “frozen” at the value of the previous stage. If a

Viscous box is selected for a particular stage, viscous stresses will be updated on that stage. If not

selected, viscous stresses will remain “frozen” at the value of the previous stage. Viscous stresses

should always be computed on the first stage, and successive evaluations will increase the “robustness”

of the solution process, but will also increase the expense (that is, increase the CPU time per iteration).

For steady problems, the final solution is independent of the stages on which viscous stresses are

updated.

.... Resetting the Multi-Stage Parameters

If you change the multi-stage parameters, but you then want to return to the default scheme set by

ANSYS Fluent, you can click the Default button in the Multi-Stage tab in the Advanced Solution

Controls Dialog Box (p. ). ANSYS Fluent will change the values to the defaults and the Default

button will become the Reset button. To get your values back again, you can click the Reset button.

The default gradient limiter in ANSYS Fluent is the Standard limiter. Each of the limiters is described

in detail in Gradient Limiters in the Theory Guide. The gradient limiters are accessible from the Expert

tab in the Advanced Solution Controls dialog box.

You can select Standard, Multidimensional, or Differentiable from the Spatial Discretization Limiter

Type drop-down list.

Each of these options can also be accessed by typing the following text command:

solve → set → slope-limiter-set

Choose from the following options:

Type

Criterion

Default (TVD) slope limiter

Multidimensional (TVD) slope limiter

Differentiable slope limiter

Note that the Default(TVD) slope limiter in the TUI is equivalent to the Standard option in

the GUI.

For each of the gradient limiter methods, ANSYS Fluent provides two limiting directions:

Selecting Gradient Limiters

Cell to Face Limiting is where the limited value of the reconstruction gradient is determined at cell face

centers.This is the default method.

Cell to Cell Limiting is where the limited value of the reconstruction gradient is determined along a scaled

line between two adjacent cell centroids. On an orthogonal mesh (or when cell-to-cell direction is parallel

to face area direction) this method becomes equivalent to the default cell to face method. For smooth field

variation, cell to cell limiting may provide less numerical dissipation on meshes with skewed cells.

ANSYS Fluent also provides the option to apply a limiter filter to the Standard and Differentiable

limiters. The purpose of the limiter filter is to maintain higher-order accuracy for the main flow variables.

It suppresses limiter intervention arising from small numerical noise, while maintaining limiter control

when there are actual discontinuities or large gradients in the solution (at shocks, boundary layers, and

so on). The limiter filter can also help in improving the apparent convergence of the solution residual.

To use the limiter filter enable Apply Limiter Filter. When the limiter filter is turned on, then by default

the filter mechanism is applied to the main flow and turbulent variables only. The filter mechanism is

based on comparing local cell changes to average global domain changes of a particular flow variable.

When the local changes are very small compared to the average global changes, then the limiter inter-

vention will be suppressed.

Note

The limiter filter is not available when using the Multidimensional limiter.

Before starting your CFD simulation, you must provide ANSYS Fluent with an initial “guess” for the

solution flow field. In many cases, you must take extra care to provide an initial solution that will allow

the desired final solution to be attained. A real-life supersonic wind tunnel, for example, will not “start”

if the back pressure is simply lowered to its operating value; the flow will choke at the tunnel throat

and will not transition to supersonic. The same holds true for a numerical simulation: the flow must be

initialized to a supersonic flow or it will simply choke and remain subsonic.

There are two methods for initializing the solution:

Initialize the entire flow field (in all cells).Three methods are available:

– Standard initialization (see Initializing the Entire Flow Field Using Standard Initialization (p. ))

– FMG initialization (see Full Multigrid (FMG) Initialization (p. ))

– Hybrid initialization (see Hybrid Initialization (p. ))

Patch values or functions for selected flow variables in selected cell zones or cell registers.

Important

Before patching initial values in selected cells, you must first initialize the entire flow field.You

can then patch the new values over the initialized values for selected variables.

If you are using one of the following in your analyses:

– user-defined real gas model (UDRGM)

– user-defined density (via UDF)

– solution-dependent expressions

then before initializing the solution using either the Hybrid Initialization method or values

from a specific zone selected in the Compute from drop-down list, you must first perform

standard initialization with no zone selected from the Compute from drop-down list.

In the first step, the standard initialization will yield the preliminary solution values, which

will be then used in the second step to obtain the desired initial values. The recommended

workflow will help resolve potential circular dependencies (such as the dependence of

solution initialization values on material properties or expressions and dependence of

material properties or expressions on solution values).

... Initializing the Entire Flow Field Using Standard Initialization

... Patching Values in Selected Cells

Before you start your calculations or patch initial values for selected variables in selected cells (Patching

Values in Selected Cells (p. )) you must initialize the flow field in the entire domain. The Solution

Initialization Task Page (p. ) (Figure . : The Solution Initialization Task Page (p. )) allows you

to set initial values for the flow variables and initialize the solution using these values.

Solution →

Initializing the Solution

You can compute the values from information in a specified zone, enter them manually, or have the

solver compute average values based on all zones. You can also indicate whether the specified values

for velocities are absolute or relative to the velocity in each cell zone. The steps for standard initialization

. Select Standard Initialization as the Initialization Method.

. Set the initial values:

To initialize the flow field using the values set for a particular zone, select the zone name in the Compute

from drop-down list. All values under the Initial Values heading will automatically be computed and

updated based on the conditions defined at the selected zone.

To initialize the flow field using computed average values, select all-zones in the Compute from drop-

down list. ANSYS Fluent will compute and update the Initial Values based on the conditions defined

at all boundary zones.

If you want to change one or more of the values, you can enter new values manually in the fields next

to the appropriate variables. If you prefer to enter all values manually, you can do so without selecting

a zone in the Compute from list. For species transport cases with a single phase flow, you can select

boundary species to be displayed in the list using the Select Boundary Species dialog box (see Fig-

ure . :The Select Boundary Species Dialog Box (p. )) that can be accessed by clicking Species in

the Solution Initialization task page.

. If your problem involves moving reference frames or sliding meshes, indicate whether the initial velocities

are absolute velocities or velocities relative to the motion of each cell zone by selecting Absolute or Rel-

ative to Cell Zone under Reference Frame. (If no zone motion occurs in the problem, the two options

are equivalent.) The default reference frame for velocity initialization in ANSYS Fluent is relative. If the

solution in most of your domain is rotating, using the relative option may be better than using the absolute

option.

. After you are satisfied with the Initial Values displayed in the task page, you can click the Initialize button

to initialize the flow field. If solution data already exist (that is, if you have already performed some calcu-

lations or initialized the solution), you must confirm that it is OK to overwrite those data.

.... Saving and Resetting Initial Values

When you initialize the solution by clicking on Initialize, the initial values will also be saved; should

you need to reinitialize the solution later, you will find the correct values in the task page when you

reopen it.

reopen it.

If you accidentally select the wrong zone from the Compute from list or manually set a value incor-

rectly, you can use the Reset button to reset all fields to their “saved” values.

Once you have initialized (or calculated) the entire flow field, you may patch different values for par-

ticular variables into different cells. If you have multiple fluid zones, for example, you may want to

patch a different temperature in each one. You can also choose to patch a custom field function

(defined using the Custom Field Function Calculator Dialog Box (p. )) instead of a constant value.

If you are patching velocities, you can indicate whether the specified values are absolute velocities or

velocities relative to the cell zone’s velocity. All patching operations are performed with the Patch

Dialog Box (p. ) (Figure . : The Patch Dialog Box (p. )).

Patch...

Solution →

Figure . : The Patch Dialog Box

. Select the variable to be patched in the Variable list.

Note

For species transport cases with a single phase flow, you can select boundary species

to be displayed in the Variable list using the Select Boundary Species dialog box (see

Figure . : The Select Boundary Species Dialog Box (p. )) that can be accessed by

clicking the Species button in the Solution Initialization task page.

. In the Zones to Patch and/or Registers to Patch lists, choose the zone(s) and/or register(s) for which you

want to patch a value for the selected variable.

Important

Important

When a shell zone has been created (that is, by enabling shell conduction for a wall and

running the calculation), the name of the shell zone will be listed in the Zones to Patch

list as shell : <wall-name>, where <wall-name> is the name of the wall in which shell

conduction has been enabled. Only temperature can be patched into the cells of a shell,

and the same value or field function will be patched into every layer of the shell.

. If you want to patch a constant value, simply enter that value in the Value field. If you want to patch a

previously-defined field function, enable the Use Field Function option and select the appropriate

function in the Field Function list.

. If you selected a velocity in the Variable list, and your problem involves moving reference frames or

sliding meshes, indicate whether the patched velocities are absolute velocities or velocities relative to

the motion of each cell zone by selecting Absolute or Relative to Cell Zone under Reference Frame. (If

no zone motion occurs in the problem, the two options are equivalent.) The default reference frame for

velocity patching in ANSYS Fluent is relative. If the solution in most of your domain is rotating, using the

relative option may be better than using the absolute option.

. Click the Patch button to update the flow-field data. (Note that patching will have no effect on the iteration

or time-step count.)

Important

If you apply a patch when setting up an ANSYS Fluent simulation from ANSYS Workbench,

the patch will not be automatically performed during future automatic solution updates

Important

from Workbench. If you need to apply the patch each time the solution is updated from

Workbench, you can do so by adding the text command /solve/patch (with appropriate

arguments) to the Original Settings command list in the Case Modification tab of the

Automatic Solution Initialization and Case Modification dialog box. See Automatic Ini-

tialization of the Solution and Case Modification (p. ) in this manual and Case Modification

Strategies with Fluent and Workbench in the Fluent in Workbench User's Guide for more

details on automatic case modification.

.... Using Registers

The ability to patch values in cell registers gives you the flexibility to patch different values within a

single cell zone. For example, you may want to patch a certain value for temperature only in fluid

cells with a particular range of concentrations for one species. You can create a cell register (basically

a list of cells) using the cell registers feature (Using Cell Registers (p. )). These functions allow you

to mark cells based on physical location, cell volume, gradient or isovalue of a particular variable

(using a field variable register), and other parameters. Once you have created a register, you can

patch values in it as described above.

.... Using Field Functions

By defining your own field function using the Custom Field Function Calculator Dialog Box (p. ),

you can patch a non-constant value in selected cells. For example, you may want to patch varying

species mass fractions throughout a fluid region. To use this feature, simply create the function as

described in Custom Field Functions (p. ), and then perform the function-patching operation in

the Patch Dialog Box (p. ), as described above.

.... Using Patching Later in the Solution Process

Since patching affects only the variables for which you choose to change the value, leaving the rest

of the flow field intact, you can use it later in the solution process without losing calculated data.

(Initialization, on the other hand, resets all data to the initial values). For example, you might want

to start a combustion calculation from a cold-flow solution. You can simply read in (or calculate) the

cold-flow data, patch a high temperature in the appropriate cells, and continue the calculation.

Patching can also be useful when you are solving a problem using a step-by-step technique, as de-

scribed in Step-by-Step Solution Processes (p. ).

For many complex flow problems such as those found in rotating machinery, or flows in expanding or

spiral ducts, flow convergence can be accelerated if a better initial solution is used at the start of the

calculation. The Full Multigrid initialization (FMG initialization) can provide this initial and approximate

solution at a minimum cost to the overall computational expense.

Full Multigrid (FMG) Initialization

For more information about FMG initialization, see Overview of FMG Initialization in the Fluent Theory

Guide.

The limitations that apply to the FMG Initialization can be found in Limitations of FMG Initialization in

Guide.

... Steps in Using FMG Initialization

... Convergence Strategies for FMG Initialization

You can access the FMG initialization procedure using the text user interface (TUI) once the standard

flow initialization is performed (see Full-Approximation Storage (FAS) Multigrid in the Theory Guide)

or if valid flow data is available (that is, through reading a data file).

To customize the FMG initialization, type the following command :

solve → initialize → set-fmg-initialization

You will be asked to enter:

The number of multigrid levels for the FMG iteration (the default is ).

Important

For small cases (,  cells or less), it is recommended that you lower the number of

multigrid levels to  or .

For each level of multigrid, you will be asked to enter the residual reduction (the default value is . ),

and the number of cycles per level (the defaults at each level are , , , , , and ). In gen-

eral, you should perform more iterations on coarse levels than fine levels. Level  is the finest level, which

represents the original mesh.

FMG iteration Courant-number (the default is . ).This will be the CFL value that the FAS multigrid will

use for the FMG initialization.

Enabling verbose mode (the default is no). By enabling this option, you will be able to monitor the conver-

gence at each level.

Important

If you do not customize the FMG settings, then the default values will be used.

To perform the FMG initialization, type the following command :

solve → initialize → fmg-initialization

Important

When you are prompted to Enable FMG initialization? [no], type yes.

When verbose mode is selected and the FMG initialization is being used, ANSYS Fluent will first output

the multigrid level information followed by convergence history for the FAS multigrid cycle on each

level. The normalized residual value is printed after ten FAS cycles or when the number of FAS cycles

is reached. The output will indicate when convergence is reached on each level and when the solution

is being interpolated to the next level.

When setting the FMG initialization parameters, you should consider performing more iterations on

the coarse levels than on the fine levels. However, remember that the purpose of FMG initialization is

to obtain a good initial solution at a low cost. You should try to avoid unreasonable convergence tol-

erance that will make the FMG initialization expensive.

Turn on the verbose mode to help you determine if the flow is converging as expected during the

FMG iterations. If the solution is not converging to the desired tolerance, consider increasing the

number of FAS multigrid cycles at each level. If the solution is diverging during the FAS cycles, then

consider lowering the FMG iteration Courant number since the default value is probably too aggressive

and is likely causing the solution to diverge.

For turbulent flows, it is very important to first perform standard initialization with proper and realistic

values of the turbulence variables (for example  and ). This can be done by computing the average

values based on the conditions defined at the inflow boundary or at all boundary zones. Then, you

can proceed with FMG initialization. Unrealistic initialization of turbulence variables may cause conver-

gence difficulties during the first few iterations on the fine mesh, thereby nullifying the benefit of FMG

Hybrid initialization is yet another initialization method in ANSYS Fluent. The other initialization methods

are standard initialization and FMG initialization. Hybrid initialization is a collection of recipes and

boundary interpolation methods. It solves Laplace's equation to determine the velocity and pressure

fields. All other variables, such as temperature, turbulence, species fractions, and volume fractions, will

be automatically patched based on domain averaged values or a particular interpolation recipe.

For more information about hybrid initialization, see Hybrid Initialization in the Theory Guide.

... Steps in Using Hybrid Initialization

... Solution Strategies for Hybrid Initialization

The default initialization method for single phase steady-state flows is the Hybrid Initialization

method.

Note

For other flow types, such as multiphase or unsteady simulations, the default initialization

method is the Standard Initialization method. However both initialization methods are

available for use in all flow conditions and types.

Hybrid Initialization

To use Hybrid Initialization, go to the Solution Initialization Task Page (p. ) (Figure . : The

Solution Initialization Task Page for Hybrid Initialization (p. )) where you will select Hybrid Initializ-

ation.

Solution →

Figure . : The Solution Initialization Task Page for Hybrid Initialization

Note

In most cases, you need not do anything more than click the Initialize button. However,

should you decide to modify the default settings for the hybrid initialization method, click

More Settings....

If you click More Settings..., the Hybrid Initialization dialog box (Figure . : The Hybrid Initialization

Dialog Box (p. )) will open. A host of settings that control the Hybrid Initialization strategy will be

available for you to adjust.

Figure . : The Hybrid Initialization Dialog Box

You can make adjustments in three different areas:

General Settings tab:

– Number of Iterations uses a default value of .This is the number of iterations that will be performed

while solving the Laplace equations to initialize the velocity and pressure. In general, you do not need

to change the number of iterations. However, for complex and highly curved geometries, if the default

number of iterations is not enough to reach the convergence tolerance of 1e- and the flow fields are

not to your liking, then you may want to increase the number of iterations and re-initialize the flow.

– Explicit Under-Relaxation Factor uses a default value of .This value will be used while solving the

Laplace equation to initialize the velocity and pressure. In general, you do not need to change the explicit

under-relaxation factor. However, for some cases, where the scalar residuals are oscillating and showing

difficulty reaching the convergence tolerance of 1e-, you may want to re-initialize the flow by reducing

the under-relaxation factor.You may also want to increase the number of iterations to produce a smooth

initialization field for the velocity and pressure.

– Reference Frame is set to Relative to Cell Zone by default. If your problem involves moving reference

frames or sliding meshes, indicate whether the initial velocities are absolute velocities or velocities relative

to the motion of each cell zone by selecting Absolute or Relative to Cell Zone. If no zone motion occurs

in the problem, the two options are equivalent. If the solution in most of your domain is rotating, using

the relative option may be better than using the absolute option.

– Initialization Options allows you to include the following options:

→ Use Specified Initial Pressure on Inlets if you want the specified pressure for Supersonic/Initialization

Gauge Pressure at the inlet boundaries to be used for solving the Laplace equation for the pressure.

Otherwise, ANSYS Fluent uses a predetermined recipe to determine the initial pressure field, as described

in Hybrid Initialization of the Theory Guide.

→ Use External-Aero Favorable Settings if you want to have the velocity potential patched with a linear

value to help accelerate convergence of Scalar Equation– and to obtain a better guess of the velocity

field for external-aero problems, such as flow over wings, airfoils, or automobiles.

→ Maintain Constant Velocity Magnitude if you want to use the flow direction obtained from solving

the velocity potential (Scalar Equation–), while maintaining a constant velocity magnitude

throughout the computational domain.This option is helpful in some incompressible external flow

problems, porous media problems, or if there are narrow channels where large undesirable velocities

can be reached.

Turbulence Settings tab uses by default the domain averaged values for the turbulence parameters. If

you want to use variable turbulence parameters you can deselect the Average Turbulent Parameters

check box.When this option is disabled, then it calculates the turbulent parameters, such as kinetic energy

and dissipation energy, using local flow parameters.

Species Settings tab will by default initialize secondary species with zero mass or mole fractions. If you

want to specify the appropriate value for the species, you will need to enable Specify Species Parameters.

Note that only the boundary species that you have selected in the Select Boundary Species dialog box

appear in the list (see Figure . :The Select Boundary Species Dialog Box (p. )).You can add or remove

a species using the Select Boundary Species that can be accessed by clicking Species in the Solution

Initialization task page.

In general, you do not need to make any extra adjustments to the hybrid initialization default settings.

However, if the hybrid initialization is not producing the initial field to your liking, then you can play

with the various options available in the Hybrid Initialization dialog box (described in Steps in Using

Hybrid Initialization (p. )), or you can also use the patching option in addition to the Hybrid Initial-

ization. For example, if you are solving a user-defined scalar, then hybrid initialization will initialize

them with a value of zero. However, you can specify the value with which you want to patch.

Note

You can also use a user-defined function to initialize the flow or certain flow variable

in conjunction with hybrid initialization.

Standard Initialization is the recommended initialization method for porous media

simulations. The default Hybrid initialization method does not account for the porous

media properties, and depending on boundary conditions, may produce an unrealistic

initial velocity field. For porous media simulations, the Hybrid initialization method

can only be used with the Maintain Constant Velocity Magnitude option.

For steady-state calculations, you will request the start of the solution process using the Run Calculation

Task Page (p. ) (Figure . : The Run Calculation Task Page (p. )).

Solution →

Here, you will supply the number of additional iterations to be performed in the Number of Iterations

field. (For unsteady calculation inputs, see User Inputs for Time-Dependent Problems (p. )). If no cal-

culations have been performed yet, ANSYS Fluent will begin calculations starting at iteration , using

the initial solution. If you are starting from current solution data, ANSYS Fluent will begin at the last it-

eration performed, using the current solution data as its starting point.

By default, ANSYS Fluent will update the convergence monitors (described in Monitoring Solution

Convergence (p. )) after each iteration. If you increase the Reporting Interval from the default of

Performing Steady-State Calculations

you can get reports less frequently. For example, if you set the Reporting Interval to , the monitors

will print or plot reports at every other iteration. Note that the Reporting Interval also specifies how

often ANSYS Fluent should check if the solution is converged. For example, if your solution converges

after  iterations, but your Reporting Interval is set to , ANSYS Fluent will continue the calculation

for an extra  iterations before checking for (and finding) convergence.

When you click the Calculate button, ANSYS Fluent will begin to calculate. While the calculation is in

progress, a progress bar will appear at the bottom of the Fluent window. For steady-state simulations,

clicking the Stop button next to the progress bar will interrupt the calculation at the earliest safe

stopping point after the current iteration. Alternatively, you can type Ctrl+c in the console. Transient

simulations have additional options for stopping, as described in User Inputs for Time-Dependent

Problems (p. ).

... Updating UDF Profiles

... Resetting Data

... Data Sampling for Steady Statistics

If you have used a user-defined function (UDF) to define any boundary conditions you can control the

frequency with which the function is updated by modifying the value of the Profile Update Interval.

If Profile Update Interval is set to , the function will be updated after every  iterations.

By default, the Profile Update Interval is set to . You might want to increase this value if your profile

computation is expensive. See the Fluent Customization Manual for details about creating and using

UDFs.

After you have performed some iterations, if you decide to start over again from the first iteration (for

example, after making some changes to the problem setup), you can reinitialize the solution using the

Solution Initialization Task Page (p. ), as described in Initializing the Entire Flow Field Using Standard

Initialization (p. ).

While notionally steady, some simulations tend to exhibit oscillatory or quasi-transient behavior. While

in principle, these simulations could be solved as unsteady flow problems and actually resolve the

transient behavior, this is often not practical and sometimes unnecessary. Data Sampling for Steady

Statistics is useful under such circumstances and helps generate averaged results and trends that are

better behaved and useful in flow predictions.

If you enable the Data Sampling for Steady Statistics option in the Run Calculation Task Page (p. )

(see Performing Steady-State Calculations (p. ) for details), ANSYS Fluent will compute the iteration

average (mean) of the instantaneous values, the root-mean-square, and the root-mean-square-errors

of those quantities and custom field functions that are enabled/selected in the Sampling Options

The Sampled Iterations field displays the iterations over which data has been sampled for the post-

processing of the mean, RMS, and RMSE values.

Use the following steps to have ANSYS Fluent gather data for steady statistics while calculating:

. (Optional) Create a custom field function for each of the variables of interest for steady statistics postpro-

cessing (for example, P*|V|) using the Custom Field Function Calculator Dialog Box (p. ). Note that

you do not need to create custom field functions for the flow shear stresses, flow heat fluxes, wall statistics, or

discrete phase variables, as these variables are available for selection later.

User Defined → Field Functions → Custom...

. Enable Data Sampling for Steady Statistics in the Run Calculation task page.

Solution →

Run Calculation →

Data Sampling for Steady Statistics

Enabling this option allows you to display and report the mean and the root-mean-square-error

(RMSE) values.

The mean, root-mean-square (RMS), and root-mean-square-error (RMSE) values for solution variables

will be available in the Steady Statistics... category (or the Steady DPM Statistics... category for

discrete phase quantities) of the variable selection drop-down list that appears in postprocessing

dialog boxes. For example, in the Contours dialog box, you could select Steady Statistics... and

RMSE-uns-custom-function- for the Contours of drop-down lists to display the root-mean-square-

errors of a custom field function named uns-custom-function-.

. Specify the Sampling Interval.

The Sampled Iterations field displays the iterations over which the data has been sampled for the

postprocessing of the mean and RMSE values.

. Select the variables for statistics sampling through the Sampling Options Dialog Box (p. ).

Solution →

. Initialize the flow statistics.

Solution → Initialization → Reset Statistics

Note that you can also reset the flow statistics after you have some data for the steady statistics. For

example, if you perform  iterations with Data Sampling for Steady Statistics enabled, check the

results, and continue with the calculation for another  iterations, the steady statistics will include the

data gathered in the first  iterations, unless you reinitialize the flow statistics.

For steady-state calculations, when using the pressure-based coupled solver or the density-based implicit

solver, you have the option of solving your flow in a pseudo-transient fashion. The pseudo transient

under-relaxation method is a form of implicit under-relaxation, described in Pseudo Transient Under-

Relaxation in the Theory Guide.

To apply the pseudo transient under-relaxation method, perform the following:

. Select the Density-Based solver or the Pressure-Based solver.

Performing Pseudo Transient Calculations

Setup →

General

. Go to the Solution Methods task page (Figure . :The Solution Methods Task Page (p. )).

Solution →

Methods

a.

Setup →

General

Solution →

Methods

a.

If you are using the pressure-based solver, the Coupled scheme under Pressure-Velocity Coupling is

b. If you are using the density-based solver, choose the Implicit scheme under Formulation.

c.

Pseudo Transient is the default option.

... Setting Pseudo Transient Explicit Relaxation Factors

In addition to pseudo transient under-relaxation, you can specify an explicit under-relaxation of the

equation to control the update of computed variables at each iteration (see Pseudo Transient Under-

Relaxation in the Theory Guide). The default values of under-relaxation parameters for all variables are

set to values that work well for most of the cases. It is good practice to start a calculation with the

default under-relaxation parameters. If your case exhibits divergence or the residuals continue to increase

after a few iterations, then you should reduce the under-relaxation factors.

You can modify the pseudo transient under-relaxation factors in the Solution Controls Task Page (p. )

(Figure . : The Solution Controls Task Page for the Pseudo Transient Runs (p. )).

Solution →

Controls

Figure . : The Solution Controls Task Page for the Pseudo Transient Runs

You can set the under-relaxation factor for each equation in the field next to its name under Pseudo

Transient Explicit Relaxation Factors.

Important

Important

... Setting Solution Controls for the Pseudo Transient Method

To have further control over the parameters for each individual equation, when solving a pseudo

transient case, you can go to the Expert tab, in the Advanced Solution Controls dialog box (Fig-

ure . : The Advanced Solution Controls Dialog Box for the Pseudo Transient Method (p. )). Note

that all equations, except for flow equations (that is pressure and momentum) will be listed. Generally,

you will not need to visit this dialog box to enter equation-specific solution parameters. However, it

may help in cases where a particular equation is giving convergence problems. Here, ANSYS Fluent

allows two options to improve convergence:

. Specify a time scale factor for the equation specific time step in lieu of using a uniform global pseudo

time step.This scaling factor scales the pseudo time step employed for the flow equations specified

in the Run Calculation task page (see Solving Pseudo-Transient Flow (p. )).

. Use the standard steady-state method by turning off pseudo transient for that particular equation.

Here, the corresponding under-relaxation factor to be employed with that equation may be specified.

The default values of under-relaxation parameters for all variables are set to values that work well

for most of the cases.

The default setting will have the pseudo transient method turned on for all equations with the corres-

ponding time scale factor set to unity, except when one of the combustion models is used. When the

pseudo transient method is enabled In combustion cases the species, enthalpy, and combustion variable

equations will only use the pseudo transient method if it is manually enabled in the Expert tab. As

well, when using the premixed, partially-premixed, or PDF combustion models, the energy equation

will only use the pseudo transient method if it is manually enabled in the Expert tab.

By default, all user-defined scalars (UDS) have pseudo transient method disabled. This is because the

physical parameters of the UDS and the appropriate time scale are not known to the solver before

starting the calculation. You can manually enable pseudo transient method for UDS under the Expert

tab in the Advanced Solution Controls Dialog Box (p. ).

Figure . : The Advanced Solution Controls Dialog Box for the Pseudo Transient Method

Specify the equation-specific steady-state solution method for a particular equation (if needed) by

enabling or disabling the pseudo transient method using the On/Off check box next to the equation.

The dialog box then allows either specification of a pseudo Time Scale Factor or Under-Relaxation

Factor for that particular equation based on the check box setting.

Note

Note

For multiphase flows, the pseudo transient expert options for the volume fraction equation

are available only when it is solved in segregated fashion. It is not available when the

Coupled with Volume Fractions option is enabled in the Solution Methods task page

(see Selecting the Pressure-Velocity Coupling Method (p. ) for information about this

setting).

... Solving Pseudo-Transient Flow

With the Pseudo Transient option enabled in the Solution Methods task page, you can now specify

the time step for the Fluid Zone and/or the Solid Zone under Pseudo Transient Settings in the Run

Calculation task page (Figure . : The Run Calculation Task Page for the User-Specified Pseudo

Transient Time Step Method (p. )).

Solution →

Figure . : The Run Calculation Task Page for the User-Specified Pseudo Transient Time Step

Method

. Select the Time Step Method for the Fluid Time Scale.

a.

If you choose User-Specified, you will enter the Pseudo Time Step, which is used for every

equation unless the equation specific time step is used for a particular equation, as mentioned

in Setting Solution Controls for the Pseudo Transient Method (p. ). Typically, the time scale

size should be relevant to the global time scale of the flow, for example:

where

is a representative length scale for the geometry (such as chord length).

b. If you use the default Automatic method (see Figure . :The Run Calculation Task Page for the

Automatic Pseudo Transient Option (p. )), the pseudo time step is calculated internally and used

for each equation listed, unless the equation has a time step specified as noted in Setting Solution

Controls for the Pseudo Transient Method (p. ).The automatic time scale is calculated from time

scales estimated for various physics active in the simulation. For more information, refer to Automatic

Pseudo Transient Time Step in the Theory Guide.

You can control the convergence process by adjusting the automatic pseudo time step value

using the Time Scale Factor field, which simply scales the calculated time step by the specified

value. The automatic time scale calculation is often somewhat conservative, and increasing the

Time Scale Factor to  or  can often increase the convergence rate. Less commonly, you

may need to reduce its value to . or . for better convergence.

Alternatively, you can also fine-tune the automatic pseudo time step by choosing the Length

Scale Method used to calculate its value. The following options are available in the drop-down

list:

Conservative: (default) uses the cube root of the mesh volume for 3D cases and square root

of area for 2D cases.

Aggressive: uses the maximum geometry extent, leading to a larger time step size than

Conservative.

User-Specified allows you to directly control the Length Scale. This method is particularly

useful in problems that have a specific length scale that is difficult to determine from

the overall geometry of the problem. For example, in the case of flow over an airfoil, the

appropriate length scale would be the length of the airfoil instead of the length scale

calculated based on the geometry of the entire domain.

You can specify the Verbosity. This is an integer value of , , or . The default value is . A

value of  prints the pseudo time step size. A value of  prints additional details about the cal-

culation.

Figure . : The Run Calculation Task Page for the Automatic Pseudo Transient Option

. Select the Time Step Method for the Solid Time Scale.

Note

Solid Time Scale only appears in the interface when a solid zone is present in the domain

or when the Energy equation is enabled along with Porous Zone or the Solidification

& Melting model.

a.

If you choose User-Specified, you will enter the Pseudo Time Step, which is used where the

Solid Time Scale is needed (that is, solid zones, porous zones, and/or solidification/melting

model).

b. If you choose Automatic, which is the default method, the pseudo time step is calculated internally

as described in Automatic Pseudo Transient Time Step in the Theory Guide. Specify a Time Scale

Factor to control/adjust the pseudo time step obtained from the automatically calculated Solid Time

Scale.

. Continue setting up your solution as you would a steady-state run, as described in Performing Steady-

State Calculations (p. ).

ANSYS Fluent can solve the conservation equations in a time-dependent manner, to simulate a wide

variety of time-dependent phenomena, such as

vortex shedding and other time-periodic phenomena

compressible filling and emptying problems

transient heat conduction

transient chemical mixing and reactions

Figure . : Time-Dependent Calculation of Vortex Shedding (t=. sec) (p. ) and Figure . : Time-

Dependent Calculation of Vortex Shedding (t=. sec) (p. ) illustrate the time-dependent vortex

shedding flow pattern in the wake of a cylinder.

Figure . : Time-Dependent Calculation of Vortex Shedding (t=. sec)

Enabling time dependence is sometimes useful when attempting to solve steady-state problems that

tend toward instability (for example, natural convection problems in which the Rayleigh number is close

to the transition region). It is possible in many cases to reach a steady-state solution by integrating the

time-dependent equations.

For details about temporal discretization, see Temporal Discretization in the Theory Guide.

... User Inputs for Time-Dependent Problems

... CFL-Based Time Stepping

... Error-Based Time Stepping

... Multiphase-Specific Time Stepping

... Postprocessing for Time-Dependent Problems

To solve a transient problem, you will follow the procedure outlined below:

. Enable the Transient option in the General task page (Figure . :The General Task Page for a Transient

Calculation (p. )).

Setup →

General

Performing Time-Dependent Calculations

Figure . : The General Task Page for a Transient Calculation

. Define all relevant models and boundary conditions. Note that any boundary conditions specified using

user-defined functions can be made to vary in time. See the Fluent Customization Manual for details.

. Specify the desired parameters in the Solution Methods task page (Figure . :The Solution Methods

Task Page for a Transient Calculation (p. )).

Solution →

Methods

Figure . : The Solution Methods Task Page for a Transient Calculation

If you are using the pressure-based solver, select PISO from the Scheme drop-down list in the

Pressure-Velocity Coupling group box. To increase the speed of the calculations, you may need

to modify the parameters related to the PISO scheme from their default values. See PISO (p. )

for more information about the optimal use of the PISO algorithm.

Important

If you are using the LES turbulence model with small time steps, the PISO scheme may

be too computationally expensive. It is therefore recommended that you select SIMPLE

or SIMPLEC instead of PISO.

Important

It is best to select the Coupled pressure-velocity coupling scheme if you are using large

time steps to solve your transient flow, or if you have a poor quality mesh.

Next, specify the desired Transient Formulation. The First Order Implicit formulation is sufficient

for most problems. If you need improved accuracy, you can either use Second Order Implicit or

Bounded Second Order Implicit. The Bounded Second Order Implicit formulation would provide

better stability, since time discretization would always ensure the bounds for variables, if available.

Important

Note that while the Bounded Second Order Implicit formulation provides the same

Important

accuracy as the Second Order Implicit formulation, it actually provides better stability.

Important

The Bounded Second Order Implicit formulation is available only for the pressure-

based solver, and not for the density-based solver.

Important

When using Second Order Implicit or Bounded Second Order Implicit formulation

for a dynamic mesh, do not run a series of simulations in which you vary the time step

size. Doing so creates an error that reduces with a reduction of the time step jump.

The Explicit formulation (available only for the density-based solver) is used primarily to capture

the transient behavior of moving waves, such as shocks. For details, see Temporal Discretization

When using the pressure-based solver, you have the additional options of selecting Non-Iterative

Time Advancement and Frozen Flux Formulation for your time-dependent flow calculations (see

Time-Advancement Algorithm and Steady-State Iterative Algorithm in the Theory Guide, respectively).

Note that the latter option is only available for single-phase transient problems that do not use a

moving/deforming mesh model.

. For transient cases that use the density-based explicit formulation, you can use the following text

command to easily switch to a two-stage Runge-Kutta scheme for the time integration. This scheme

results in faster calculations than the default three- or four-stage Runge-Kutta scheme (especially

for laminar flows), though the reduced stability range may require changes to the setup as described

below.

below.

> solve/set/fast-transient-settings/rk2

Enable two-stage Runge-Kutta scheme? [no] yes

This text command will set the Number of Stages to  in the Multi-Stage tab of the Advanced

Solution Controls Dialog Box (p. ), with coefficients of . and . For further details about these

settings, see Setting Multi-Stage Time-Stepping Parameters (p. ). If your solution diverges with

this scheme, you can attempt the calculation again with a lower Courant number (typically less

than ) and, for implicit time stepping, a higher value for the maximum number of iterations per

time step; if necessary, you can use the rk2 text command again to easily disable the two-stage

Runge-Kutta scheme and revert back to the default multi-stage scheme for your time-stepping

scheme (summarized in Summary of the Density-Based Solver in the Fluent Theory Guide).

. (optional) If you are using the explicit transient formulation with specified Courant number or if

you are using any of the adaptive time stepping methods (described in a later step) it is recommen-

ded that you enable the printing of the current time (for the explicit transient formulation) or the

current time step size (for the adaptive time stepping method) at each iteration, using Fig-

ure . : Report File for 'flow-time', 'delta-time', and 'iters-per-timestep' (p. ).

Solution → Monitors → Statistic

Edit...

Make sure that the desired item is selected from the Statistics selection list (time for the current

time or delta_time for the current time step size) and enable the Print option. When ANSYS Flu-

ent prints the residuals to the console at each iteration, it will include a column with the current

time or the current time step size.

. (optional) Use the Drag Report Definition Dialog Box (p. ), the Lift Report Definition Dialog Box (p. ),

the Moment Report Definition Dialog Box (p. ), or the Surface Report Definition Dialog Box (p. ) to

monitor (and/or save to a file) time-varying force coefficient values or a report of a field variable or function

on a surface as it changes with time. See Monitoring Solution Convergence (p. ) for details.

. Set the initial conditions (at time

) using the Solution Initialization task page.

Solution →

You can also read in a steady-state data file to set the initial conditions.

. Use the Autosave dialog box to specify the file name and frequency with which case and data files should

be saved during the solution process.To open the Autosave dialog box, click the Edit... button next to

Autosave Every in the Calculation Activities task page.

On

See Automatic Saving of Case and Data Files (p. ) for details about automatic file saving.

The Calculation Activities task page also allows you to export solution and particle history data

during the transient calculation. See Exporting Data During a Transient Calculation (p. ) for details.

If you want to create a graphical animation of the solution over time, you can use Figure . : The

Animation Definition Dialog Box (p. ) to set up the graphical displays that you want to use in

the animation. See Animating the Solution (p. ) for details.

You may also want to request automatic execution of other commands using the Execute Commands

Dialog Box (p. ). See Executing Commands During the Calculation (p. ) for details.

. Specify time-dependent solution parameters and start the calculation as described below for the implicit

and explicit transient formulations:

If you have chosen the First Order Implicit, Second Order Implicit, or Bounded Second Order Implicit

formulation, the procedure is as follows:

a.

Open the Run Calculation Task Page (p. ) (see Figure . :The Run Calculation Task Page for

Implicit Transient Calculations (p. )).

Solution →

Figure . : The Run Calculation Task Page for Implicit Transient Calculations

b. If you want the time steps to remain a fixed size throughout the simulation, select Fixed from the

Type drop-down list, and then select one of the following from the Method drop-down list:

– User-Specified: with this method, you will specify the desired Number of Time Steps and the

Time Step Size.

– Period-Based or Frequency-Based: these methods are convenient when setting up unsteady

turbomachinery cases or any case that exhibits transient periodic behavior.They allow you to

define the setup in terms of the Period or Frequency, the Time Steps per Period, and the Total

Periods, and then Fluent will automatically set an appropriate Time Step Size and Number of

Time Steps.

When ANSYS Fluent solves the time-dependent equations using the implicit formulation,

multiple iterations may be necessary at each time step, so you can specify a value for the

Max Iterations/Time Step you would like to allow. If the convergence criteria are met

before this number of iterations is performed, the solution will advance to the next time

step.

The time step size is the magnitude of

. Since the ANSYS Fluent formulation is fully implicit,

there is no stability criterion that must be met in determining

. However, to model transient

phenomena properly, it is necessary to set

at least one order of magnitude smaller than

the smallest time constant in the system being modeled. A good way to judge the choice of

is to observe the number of iterations ANSYS Fluent needs to converge at each time step.

The ideal number of iterations per time step is –. If ANSYS Fluent needs substantially

more, the time step is too large. If ANSYS Fluent needs only a few iterations per time step,

should be increased. Frequently a time-dependent problem has a very fast “startup”

transient that decays rapidly. Therefore, it is often wise to choose a conservatively small

for the first – time steps.

may then be gradually increased as the calculation proceeds.

For time-periodic calculations, you should choose the time step based on the time scale of

the periodicity. For a rotor/stator model, for example, you might want  time steps between

each blade passing. For vortex shedding, you might want  steps per period.

To verify that your choice for

was proper after the calculation is complete, you can plot

contours of the Courant number within the domain. To do so, select Velocity... and Cell

Convective Courant Number from the Contours of drop-down lists in the Contours dialog

box. For a stable, efficient calculation, the Courant number should not exceed a value of

– in most sensitive transient regions of the domain.

Note

The Period-Based and Frequency-Based methods are not available for in-cylinder

dynamic mesh simulations; instead, the User-Specified method must be used,

and the time step size will be computed based on the crank shaft speed and the

crank angle step size.

c.

If you want ANSYS Fluent  to modify the size of the time step as the calculation proceeds, select

Adaptive from the Type drop-down list, and then select one of the following from the Method

drop-down list:

– CFL-Based: with this method, ANSYS Fluent will modify the size of the time step as the

calculation proceeds such that the Courant–Friedrichs–Lewy (CFL) condition is satisfied.

See CFL-Based Time Stepping (p. ) for details.

– Error-Based: with this method, the time step is modified by ANSYS Fluent  based on the specified

truncation Error Tolerance. See Error-Based Time Stepping (p. ) for details.

– Multiphase-Specific: with this method, the time step is modified by ANSYS Fluent  based on the

convective time scale (Global Courant Number).The time step size calculation depends on the

mesh density and velocity in interfacial cells.This method is available for all multiphase models

using implicit or explicit volume fraction formulation, except for the wet steam model. See Mul-

tiphase-Specific Time Stepping (p. ) for details.While this method and the CFL-Based approach

both use a Courant number, they differ in that the Multiphase-Specific method considers the

interface regions when computing the time step size, whereas the CFL-Based method is based

on a global time marching approach.

Note

The Adaptive type is not available for simulations that use the acoustic model

and/or the structural model. It is also unavailable for in-cylinder dynamic mesh

simulations; in this case, the fixed User-Specified method must be used, and the

time step size will be computed based on the crank shaft speed and the crank

angle step size.

Next, make a selection from the Duration Specification Method drop-down list in order to

specify the way in which you will define the calculation duration. The duration can be defined

by the total time, the total number of time steps, the incremental time, or the number of

incremental time steps. In this context, "total" indicates that Fluent will consider the amount

of time / steps that have already been solved and stop appropriately, whereas "incremental"

indicates that the solution will proceed for a specified amount of time / steps regardless of

what has previously been calculated.

It is a good idea to perform a few fixed-size time steps before switching to the adaptive time

stepping. Sometimes spurious discretization errors can be associated with an impulsive start

in time. These errors are dissipated during the first few time steps, but they can adversely

affect the adaptive time stepping and result in extremely small time steps at the beginning

of the calculation. You can specify the Number of Fixed Time Steps that should be performed

before the size of the time step starts to change. The size of the fixed time step is the value

specified for Initial Time Step Size; this value must fall between the minimum and maximum

time step sizes. For a better startup, it should be chosen such that the Courant number initially

remains close to  or your specified value (whichever is lower). Note that if you initialize the

solution for a previously run case with adaptive time stepping, then ANSYS Fluent will use

the time step size saved in the case.

Important

When the solution tends to exhibit incomplete convergence for the Error-Based

method, rather than increasing the time step size or keeping the same time step

size in the next step, ANSYS Fluent reduces the time step size for the next time

step (making sure that the time step size does not go below the specified minimum

time step size).

Max Iterations/Time Step you would like to allow. If the convergence criteria are met before

this number of iterations is performed, the solution will advance to the next time step. You

can also define the Time Step Size Update Interval, which specifies the number of time

steps that will pass before the time step size is updated for adaptive time stepping methods.

Finally, click the Settings... button and complete the setup for the adaptive time stepping

method in the Adaptive Time Stepping Dialog Box (p. ), setting the minimum / maximum

time step sizes and change factors.

Tip

If you need your simulation to end exactly at your specified total or incremental

time, input smaller and smaller values for the minimum time step size until this

condition is met.

d. If you want to define your own adaptive time stepping method rather than use one of the

Adaptive types described previously, you can create a user-defined function for your method

using the DEFINE_DELTAT macro. After you have compiled or interpreted it, you can select

User-Defined Function from the Type drop-down list and then select it from the User-

Defined Time Step drop-down list. You can then define the duration method and time /

number of time steps, as described previously for the Adaptive types.

See the Fluent Customization Manual for details about creating and using user-defined

e. (optional) You can improve the convergence of the transient calculations by enabling the Extrapolate

Variables option in the Run Calculation Task Page (p. ).This option instructs ANSYS Fluent to

predict the solution variable values for the next time step using a Taylor series expansion, and then

inputs that predicted value as an initial guess for the inner iterations of the current time step. As a

result, the absolute residual levels are lowered.

Note that the Extrapolate Variables option is not available if you are employing either the

NITA scheme with the pressure-based solver or the explicit formulation with the density-

Important

If you use the Extrapolate Variables option when modeling an incompressible

flow with the density-based solver, it is recommended that you disable the extra-

polation of pressure values. After you have enabled the Extrapolate Variables

option, type the following text command in the console:

> solve/set/extrapolate-eqn-vars/pressure

Extrapolate Pressure? [yes] no

f.

To view details about the time advancement of the simulation, enable the Report Simulation Status

option in the Options group box.While this option is enabled (before, after, or during a calculation),

the Simulation Status Dialog Box (p. ) will be open and reporting information.

g. (optional) If you want ANSYS Fluent to gather data for time statistics (that is, time-averaged, root-

mean-square, and root-mean-square-error values for solution variables) during the calculation, follow

these steps:

i.

Create a custom field function for the each of the variables for which you want to post-

process unsteady statistics (for example, P*|V|), using the Custom Field Function Calcu-

lator. For detailed instructions, see Creating a Custom Field Function (p. ). Note that

you do not need to take the extra step of creating custom field functions for the flow

shear stresses, flow heat fluxes, wall statistics, or discrete phase variables as there are

options for selecting these variables directly in a later step.

Parameters & Customization → Custom Field Functions

New...

Important

New...

Important

The maximum number of custom field functions that can be calculated and

postprocessed for unsteady statistics is .

ii.

Enable the Data Sampling for Time Statistics option in the Run Calculation Task Page (p. ).

Solution →

Data Sampling for Time Statistics

Enabling this option will allow you to display and report the mean, the root-mean-square

(RMS), and the root-mean-square-error (RMSE) values, as described in Postprocessing for

Time-Dependent Problems (p. ).

To specify the sampling interval, enter a value for Sampling Interval.

The Sampled Time displays the time period over which data has been sampled for the

postprocessing of the mean, RMS, and RMSE values. For most quantities, as long as the

time step size has been constant, dividing this by the time step size yields the number

of data sets that have been collected. However, special consideration is required in the

case of discrete phase quantities. As noted in Reporting of Unsteady DPM Statistics (p. ),

sampling of DPM quantities occurs only when parcels pass through a cell, not necessarily

at each specified sampling interval. Therefore, the number of samples of the DPM

quantities taken during the sampled time period is stored in the separate postprocessing

variable, Accum DPM Parcels in Cell. If the time step size is varied, every contribution

To select the variables (which may be represented as custom field functions) for which

you want to collect statistics, click the Sampling Options... button and make selections

from the Sampling Options dialog box that opens (Figure . : The Sampling Options

Dialog Box (p. )). Note that no custom field functions are selected by default.

Solution →

Important

Note that gathering data for time statistics is not meaningful inside a moving

cell zone (for example, a sliding zone in a sliding mesh problem, a moving

zone in a dynamic mesh problem).

iii. Initialize the flow statistics.

Reset Statistics

Note that you can also reset the flow statistics after you have gathered some data for

time statistics. If you perform, say,  time steps with the Data Sampling for Time Stat-

istics option enabled, check the results, and then continue the calculation for  more

time steps, the time statistics will include the data gathered in the first  time steps unless

you reinitialize the flow statistics.

h. Click the Calculate button. As it calculates a solution, ANSYS Fluent will print the current time at

the end of each time step.

If you choose the Explicit transient formulation,you have two input options available for specifying

the transient solution advancement: you can specify the transient advancement either directly by spe-

cifying a time step size (

) or indirectly via entering a Courant number value (

) in the Solution

Controls task page.The steps for these two options are as follows:

– If the default option Specified Time Step is enabled in the Solution Controls task page, you will be

required to specify the time advancement settings in the Run Calculation task page: you need to

define the time stepping as either a Fixed or User-Defined Function type (as described previously

for the implicit formulations) and click the Calculate button.

Note

The stability of an explicit formulation is limited by the Courant-Fredrichs-Lewy

condition. Fluent checks the specified time step against the stability limit. The sta-

bility limit is the maximum allowable time step size calculated based on

in

Equation . (p. ). The stability limit is also the minimum of all local time steps

in the domain. If the specified time step size is larger than the maximum allowable

time step, Fluent displays a warning during the calculation.

– If you disable the Specified Time Step option, you will be required to specify the Courant Number

in the Solution Controls task page.Then you can define the Number of Time Steps in the Run

Calculation task page and click Calculate. In this option the (

) value is used to calculate the time

step size (

) using Equation . (p. ):

(.)

where,

is the volume of the cell,

is the face area, and

is the maximum local eigen-

value defined in Equation . in the Fluent Theory Guide.

When you click the Calculate button, ANSYS Fluent will begin to calculate. While the calculation

is in progress, a progress bar will appear at the bottom of the Fluent window. For transient simula-

tions, clicking the buttons next to the progress bar will interrupt the calculation at the earliest safe

stopping point: you can choose to stop the calculation at the end of either the current iteration

or current time step. Alternatively, you can type Ctrl+c in the console: a single instance will stop

the calculation at the end of the current time step, whereas typing it twice will stop it at the end

of the current iteration.

You can access the information saved in a data file, which includes a standard set of quantities

that were computed during the calculation, by clicking the Data File Quantities... button. More

information about this feature is available in Setting Data File Quantities (p. ).

. Save the final data file (and case file, if you have modified it) so that you can continue the transient calcu-

lation later, if desired.

.... Additional Inputs

The procedures for setting the reporting interval, updating user-defined function profiles, interrupting

iterations, and resetting data are the same as those for steady-state calculations. See Performing

Steady-State Calculations (p. ) for details.

Important

If you are using a user-defined function in your time-dependent calculation, note that, in

addition to being updated after every  iterations (where  is the value of the Profile

Update Interval), the function will also be updated at the first iteration of each time step.

As mentioned in User Inputs for Time-Dependent Problems (p. ), it is possible to have the size of

the time step change as the calculation proceeds such that the Courant–Friedrichs–Lewy (CFL) condition

is satisfied. Note that the time step size will only vary if the solution of the flow equation is enabled,

and it is a convection-dominant flow. This section provides a brief description of the algorithm that

ANSYS Fluent uses to compute the time step size, as well as an explanation of parameters that you

can set to control the CFL-based time stepping.

Important

CFL-based time stepping is available only with the pressure-based and density-based implicit

formulations; it cannot be used with the density-based explicit formulation. Also, it cannot

be used with multiphase flows, the in-cylinder dynamic mesh option, the acoustic model,

and/or the structural model, nor is it available with the second-order implicit formulation

if the fixed time step formulation is selected through the solve/set/second-order-

time-options text command or through the enabling of a dynamic mesh.

Note

If there are other time scales controlling the physics of problem (surface tension time scale,

meshing-driven time scales for mesh deformation, and so on), then the CFL-based time

stepping is not a good choice.

....The CFL-Based Time Stepping Algorithm

For a cell

, a local time step size is calculated based on the Courant number (

) that you have

defined as part of the settings:

(.)

where

(.)

(.)

and

= Cell volume

= Constant factor

= Inviscid spectral radii

= Viscous spectral radii

= Surface area vector

= Number of cell faces

The global time step size is then defined as the minimum local time step size in the domain, provided

that it is within the minimum and maximum values that you have defined as part of the settings.

.... Specifying Parameters for CFL-Based Time Stepping

For transient flows, when you select Adaptive for the Type and CFL-Based for the Method in the

Run Calculation task page, you can then set the time stepping parameters as described in User Inputs

for Time-Dependent Problems (p. ). The following provides further details that are specific for the

CFL-based time stepping.

In the Run Calculation task page:

is

in Equation . (p. ), which represents the ratio of the time step size to the characteristic time

taken for the fluid to cross a control volume. For convection-dominant and/or wave propagation problems,

it is recommended that you set this close to  in order to obtain more accurate results. Increasing it will

result in an increase of the time step size and consequently a faster transient simulation; however, this

may have a negative impact on the convergence, stability, and accuracy of your transient simulation.

Initial Time Step Size

is used for the first time step and then for as many subsequent steps as specified in the Number of Fixed

Time Steps field.This value must fall between the minimum and maximum time step sizes. It should be

chosen such that the Courant Number initially remains close to  or your specified value (whichever is

lower) for a better startup. Note that if you initialize the solution for a previously run case with adaptive

time stepping, then ANSYS Fluent will use the time step size saved in the case file.

In the Adaptive Time Stepping dialog box:

Minimum / Maximum Step Change Factor

limit the degree to which the time step size can change at each time step. Limiting the change results

in a smoother calculation of the time step size, especially when high-frequency noise is present in the

solution.The time step change factor is computed as the ratio between the current time step and the

previous time step.

When choosing the values, it is generally not recommended to allow large variation in time step

size due to stability considerations. This is especially true when the time step size is ramping up.

It is recommended that you use a minimum time step size factor in the range of . to ., and

a maximum time step change factor in the range of . to . The default values of . and , re-

spectively, provide a smooth transition of the time step size.

the time step change as the calculation proceeds based on the truncation error tolerance. This section

provides a brief description of the algorithm that ANSYS Fluent uses to compute the time step size,

as well as an explanation of parameters that you can set to control the error-based time stepping.

Important

Error-based time stepping is available only with the pressure-based and density-based im-

plicit formulations; it cannot be used with the density-based explicit formulation. It cannot

be used with second-order time integration and/or the in-cylinder dynamic mesh option;

it is also unavailable with Euler-Euler multiphase models (described in Approaches to Mul-

tiphase Modeling in the Theory Guide), with the exception of the Eulerian model when the

implicit volume fraction formulation is enabled.

....The Error-Based Time Stepping Algorithm

The automatic determination of the time step size is based on the estimation of the truncation error

associated with the time integration scheme. If the truncation error is smaller than a specified tolerance,

the size of the time step is increased; if the truncation error is greater, the time step size is decreased.

An estimation of the truncation error can be obtained by using a predictor-corrector type of algorithm

[] (p. ) in association with the time integration scheme. At each time step, a predicted solution

can be obtained using a computationally inexpensive explicit method: forward Euler for the first-order

unsteady formulation. This predicted solution is used as an initial condition for the time step, and

the correction is computed using the nonlinear iterations associated with the implicit (pressure-based

or density-based) formulation. The norm of the difference between the predicted and corrected

solutions is used as a measure of the truncation error. By comparing the truncation error with the

desired level of accuracy (that is, the truncation error tolerance), ANSYS Fluent is able to adjust the

time step size by increasing it or decreasing it.

In cases where the truncation error remains above the specified tolerance, ANSYS Fluent will try to

meet the tolerance within  attempts. If this tolerance is met or the  attempts are completed, then

the iteration moves on to the next time step. An explicit scheme is used to predict the solution at

each time step, then the explicit prediction is corrected with an implicit scheme. The truncation error,

which is a function of the difference between the predicted and corrected solutions at a specific time

is used to calculate the next time step. However, if the calculated truncation error is greater than the

tolerance limit, we have the option of reverting from the currently performed iteration, which is

moving from the

th step to

th step, and performing the iteration with a smaller time step. Since

the truncation error is proportional to the time step, decreasing the time step reduces the truncation

error. This can be done until the truncation error goes below the tolerance limit.

.... Specifying Parameters for Error-Based Time Stepping

For transient flows, when you select Adaptive for the Type and Error-Based for the Method in the

error-based time stepping.

specifies the threshold value to which the computed truncation error is compared. Increasing this value

will lead to an increase in the size of the time step and a reduction in the accuracy of the solution. De-

creasing it will lead to a reduction in the size of the time step and an increase in the solution accuracy,

although the calculation will require more computational time. For most cases, the default value of .

is acceptable.

chosen such that the Courant number initially remains close to  for a better startup. Note that if you

initialize the solution for a previously run case with adaptive time stepping, then ANSYS Fluent will use

the time step size saved in the case file.

Minimum/Maximum Step Change Factor

solution. If the time step change factor,

, is computed as the ratio between the specified truncation

error tolerance and the computed truncation error, the size of time step

is computed as follows:

If

,

is increased to meet the desired tolerance.

If

,

is increased, but its maximum possible value is

.

If

,

is unchanged.

If

,

is decreased.

Multiphase-specific time stepping is supported for all multiphase models using implicit or explicit

volume fraction formulation, except for the wet steam model. It is not supported with the in-cylinder

dynamic mesh option, the acoustic model, and/or the structural model.

Multiphase-specific time stepping is based on the convective time scale (Courant based), in which the

time-step-size calculation depends on the mesh density and velocity in interfacial cells.

Note

meshing-driven time scales for mesh deformation, and so on), then the Courant-based time

scale is not a good choice.

....The Multiphase-Specific Time Stepping Algorithm

The global time step

is changed in the following manner:

(.)

where

is the global Courant number, and the ratio

is calculated for each

cell. ANSYS Fluent takes the maximum of this ratio to calculate the global time step.

.... Specifying Parameters for Multiphase-Specific Time Stepping

For transient flows, when you select Adaptive for the Type and Multiphase-Specific for the Method

in the Run Calculation task page, you can then set the time stepping parameters as described in

User Inputs for Time-Dependent Problems (p. ). The following provides further details that are

specific for the multiphase-specific time stepping.

Global Courant Number

is the ratio of the time step size to the characteristic time taken for the fluid to cross a control volume.

To calculate the Courant number, ANSYS Fluent uses a flux-based definition where, in the region near

the fluid interface, ANSYS Fluent divides the volume of each cell by the sum of the outgoing fluxes.The

resulting time represents the time it would take for the fluid to empty out of the cell.The smallest such

time is used as the characteristic time of transit for a fluid element across a control volume.The default

value for Global Courant Number is , which means that the estimated time step size is twice the

characteristic time of transit.

The optimal value for Global Courant Number is dependent on a specific case. The general re-

commendations on choosing an appropriate value for Global Courant Number are summarized

below.

Explicit volume fraction formulation

– For accuracy of an instantaneous-time solution, the default value of  is recommended.

– For a time-averaged solution, you can use higher values, but not larger than .

Implicit volume fraction formulation

– For an instantaneous-time solution, you can set Global Courant Number to  (recommended) with

the first order time formulation and to a higher value (up to ) with the second order time formula-

tion.

– For a time-averaged solution, you can use even higher values (up to ).

chosen such that the Global Courant Number initially remains close to  or your specified value

(whichever is lower) for a better startup. Note that if you initialize the solution for a previously run case

with adaptive time stepping, then ANSYS Fluent will use the time step size saved in the case file.

size due to stability considerations. This is especially true when time step size is ramping up. It is

recommended that you use a minimum time step size factor in the range of . to . and a

maximum time step change factor in the range of . to .. The default values of . and .,

respectively, provide a smooth transition of the time step size.

The postprocessing of time-dependent data is similar to that for steady-state data, with all graphical

and alphanumeric commands available. You can read a data file that was saved at any point in the

calculation (by you or with the autosave option) to restore the data at any of the time levels that were

saved.

ANSYS Fluent will label any subsequent graphical or alphanumeric output with the time value of the

current data set.

If you save data from the force or surface report definitions to files (see step  in User Inputs for Time-

Dependent Problems (p. )), you can read these files back in and plot them to see a time history of

the monitored quantity. Figure . : Lift Coefficient Plot for a Time-Periodic Solution (p. ) shows a

sample plot generated in this way.

If you enable the Data Sampling for Time Statistics option in the Run Calculation Task Page (p. )

(see Performing Time-Dependent Calculations (p. ) for details), ANSYS Fluent will compute the time

The Sampled Time displays the time over which data has been sampled for the postprocessing of the

mean, RMS, and RMSE values. For most quantities, as long as the time step size has been constant,

dividing this by the time step size yields the number of data sets that have been collected. However,

special consideration is required In the case of discrete phase quantities. As noted in Reporting of

Unsteady DPM Statistics (p. ), sampling of DPM quantities occurs only when parcels pass through

a cell, not necessarily at each specified sampling interval. Therefore, the number of samples of the

DPM quantities taken during the sampled time period is stored in the separate postprocessing variable,

Accum DPM Parcels in Cell. If the time step size is varied, every contribution of data sets sampled is

automatically weighted by the current time step size.

The mean, root-mean-square(RMS), and root-mean-square-error (RMSE) values for solution variables

will be available in the Unsteady Statistics... category (or the Unsteady DPM Statistics... category

for discrete phase quantities) of the variable selection drop-down list that appears in postprocessing

dialog boxes. For example, in the Contours dialog box, you could select Unsteady Statistics... and

RMSE-uns-custom-functon- for the Contours of drop-down lists in order to display the root-mean-

square-errors of a custom field function named uns-custom-functon-.

During the solution process you can monitor the convergence dynamically by checking residuals, stat-

istics, force values, surface integrals, and volume integrals. You can print reports of or display plots of

lift, drag, and moment coefficients, surface integrations, and residuals for the solution variables. For

unsteady flows, you can also monitor elapsed time. Creating report definitions for monitoring is described

in Creating Report Definitions (p. ).

... Monitoring Residuals

... Monitoring Statistics

... Monitoring Solution Quantities

At the end of each solver iteration, the residual sum for each of the conserved variables is computed

and stored, thereby recording the convergence history. This history is also saved in the data file. The

residual sum is defined below.

On a computer with infinite precision, these residuals will go to zero as the solution converges. On an

actual computer, the residuals decay to some small value (“round-off”) and then stop changing (“level

out”). For single-precision computations (the default for workstations and most computers), residuals

can drop as many as six orders of magnitude before hitting round-off. Double-precision residuals can

drop up to twelve orders of magnitude. Guidelines for judging convergence can be found in Judging

Convergence (p. ).

.... Definition of Residuals for the Pressure-Based Solver

After discretization, the conservation equation for a general variable

at a cell  can be written as

(.)

Here

is the center coefficient,

are the influence coefficients for the neighboring cells, and  is

the contribution of the constant part of the source term

in

and of the boundary condi-

tions. In Equation . (p. ),

(.)

The residual

computed by ANSYS Fluent’s pressure-based solver is the imbalance in Equa-

tion . (p. ) summed over all the computational cells . This is referred to as the “unscaled” re-

sidual. It may be written as

(.)

In general, it is difficult to judge convergence by examining the residuals defined by Equa-

tion . (p. ) since no scaling is employed. This is especially true in enclosed flows such as natural

convection in a room where there is no inlet flow rate of

with which to compare the residual.

ANSYS Fluent scales the residual using two kinds of scaling factors, representative of the flow rate of

through the domain. The factors are termed global scaling and local scaling. The type of scaling

can be selected from the Residual Monitors dialog box. The “globally scaled” residual is defined as

(.)

There are two instances where

is modified in the denominator term

: for momentum equations,

it is replaced with the magnitude of the velocity at cell ; and for Reynold stress equations, it is re-

Monitoring Solution Convergence

placed with the trace of the Reynolds stress tensor at cell  divided by the number of dimensions of

the case (2D or 3D).

The “locally scaled” residual is defined as

(.)

Note that for the momentum and Reynolds stress equations,

(.)

and

are modified in the same

manner as for global scaling.

The scaled residual is a more appropriate indicator of convergence for most problems. The selection

of scaling and convergence criteria for different types of scaling are discussed in Judging Conver-

gence (p. ). The default residuals displayed by ANSYS Fluent are global scaling.

For the continuity equation, the unscaled residual for the pressure-based solver is defined as

(.)

The local scaling is the same for all equations. However, the global scaling treats continuity in a dif-

ferent way and it is defined as

(.)

The denominator is the largest absolute value of the continuity residual in the first five iterations.

The scaled residuals described above are useful indicators of solution convergence. Guidelines for

their use are given in Judging Convergence (p. ). It is sometimes useful to determine how much

a residual has decreased during calculations as an additional measure of convergence. For this purpose,

ANSYS Fluent allows you to normalize the residual (either scaled or unscaled) by dividing by the

maximum residual value after

iterations, where

is set by you in the Residual Monitors Dialog

Box (p. ) in the Iterations field under Residual Values.

(.)

Normalization in this manner ensures that the initial residuals for all equations are of

and is

sometimes useful in judging overall convergence.

. You can also specify the normalization factor (the denominator in Equa-

tion . (p. )) manually in the Residual Monitors Dialog Box (p. ).

.... Definition of Residuals for the Density-Based Solver

A residual for the density-based solver is simply the time rate of change of the conserved variable

(

). The RMS residual is the square root of the average of the squares of the residuals in each cell

of the domain:

(.)

Equation . (p. ) is the unscaled residual sum reported for all the coupled equations solved by

ANSYS Fluent’s density-based solver.

Important

The residuals for the equations that are solved sequentially by the density-based solver

(turbulence and other scalars, as discussed in Density-Based Solver in the Theory Guide)

are the same as those described above for the pressure-based solver.

with which to compare the residual. As

with the pressure-based solver, ANSYS Fluent uses two types of scaling for the density-based solver.

The globally scaled residual is defined as

(.)

The denominator is the largest absolute value of the residual in the first five iterations.

The locally scaled residual is calculated from the local flux imbalance in the cell. It is calculated using

Equation . (p. ):

(.)

is the conservative variable and

is the cell volume. The unscaled residual is always calculated

from Equation . (p. ).

Normalization of the residual sum is accomplished by dividing by the maximum residual value after

is set by you in the Residual Monitors Dialog Box (p. ) in the Iterations field

under Residual Values:

(.)

and is

, making the normalized residual equivalent to the scaled residual. You can also

specify the normalization factor (the denominator in Equation . (p. )) manually in the Residual

Monitors Dialog Box (p. ).

.... Overview of Using the Residual Monitors Dialog Box

All inputs controlling the monitoring of residuals are entered using the Residual Monitors Dialog

Box (p. )(Figure . : The Residual Monitors Dialog Box (p. )).

Edit...

Figure . : The Residual Monitors Dialog Box

In general, you will only need to enable residual plotting and modify the convergence criteria using

this dialog box. Additional controls are available for disabling monitoring of particular residuals, and

modifying normalization and plot parameters.

.... Printing and Plotting Residuals

By default, residual values for all relevant variables are printed in the console after each iteration. If

you want to disable this printout, turn off Print to Console under Options. To enable the plotting

of residuals after each iteration, turn on Plot under Options. Residuals will be plotted in the graphics

window (with the window ID set in the Window field) during the calculation.

If you want to display a plot of the current residual history, simply click the Plot push button.

.... Storing Residual History Points

Residual histories for each variable are automatically saved in the data file, regardless of whether they

are being monitored. You can control the number of history points to be stored by changing the It-

erations to Store entry. By default, up to  points will be stored. If more than  iterations are

performed (that is, the limit is reached), every other point will be discarded—leaving  history

points—and the next  points will be stored. When the total hits  again, every other point will

again be discarded, and so on. If you are performing a large number of iterations, you will lose a

great deal of residual history information at the beginning of the calculation. In such cases, you should

increase the Iterations to Store value to a more appropriate value. Of course, the larger this number

is, the more memory you will need, the longer the plotting will take, and the more disk space you

will need to store the data file.

.... Controlling Normalization and Scaling

By default, scaling of residuals (see Equation . (p. ) and Equation . (p. )) is enabled and

the default convergence criterion is

for energy and P- equations and

for all other equations.

When the Scale option is enabled, global scaling will be applied by default. You can then enable the

Compute Local Scale option and select the Reporting Option from the drop-down list. You have a

choice to plot or print to the console the local scaling or the global scaling of residuals. By default,

the global scaling of residuals will be plotted.

Note

When Compute Local Scale is enabled, ANSYS Fluent computes and stores both the

locally and globally scaled residuals from subsequent iterations, for the purpose of

reporting. The scaled residuals are stored in the data file.

Important

Once the Compute Local Scale option is enabled and you disable the Scale option,

the Compute Local Scale option will not automatically be disabled. Instead, it will

compute both the locally and globally scaled residuals, but only print or plot the un-

scaled residual.

Residual normalization (that is, dividing the residuals by the largest value during the first few iterations)

is also available but disabled by default.

Normalization can be used with both scaled and unscaled residuals. Note that if normalization is en-

abled, the convergence criterion may need to be adjusted appropriately. See Judging Conver-

gence (p. ) for information about judging convergence based on the different types of residual

reports. (Both the raw residuals and scaling factors are stored in the data file, so you can switch

between scaled and unscaled residuals.)

To report unscaled residuals, simply disable the Scale option under Residual Values.

Important

If you switch from scaled to unscaled residuals (or vice versa) and you are normalizing the

residuals (as described below), you must click the Renormalize button to recompute the

normalization factors.

If you want to normalize the residuals (see Equation . (p. ) or Equation . (p. )), enable

the Normalize option under Residual Values. The Normalization Factor column will be added to

the dialog box at this time. ANSYS Fluent will normalize the printed or plotted residual for each variable

by the value indicated as the Normalization Factor for that variable. The default Normalization

Factor is the maximum residual value after the first  iterations. To use the maximum residual value

after a different number of iterations (that is, specify a different value for

or Equation . (p. )), you can modify the Iterations entry under Residual Values.

In some cases, the maximum residual may occur sometime after the iteration specified in the Iterations

field. If this should occur, you can click the Renormalize button to set the normalization factors for

all variables to the maximum values in the residual histories. Subsequent plots and printed reports

will use the new normalization factor.

You can also specify the normalization factor (the denominator in Equation . (p. ) or Equa-

tion . (p. )) explicitly. To modify the normalization factor for a particular variable, enter a new

value in the corresponding Normalization Factor field in the Residual Monitors Dialog Box (p. ).

If you want to report unnormalized, unscaled residuals (Equation . (p. ) or Equation . (p. )),

disable the Normalize and Scale options under Residual Values in the Residual Monitors Dialog

Box (p. ). Note that unnormalized, unscaled residuals are stored in the data file regardless of

whether the reported residuals are normalized or scaled.

.... Choosing a Convergence Criterion

The ability to choose certain convergence criteria provides you with alternative ways to check conver-

gence when using the iterative transient solver. The various convergence criteria can be selected in

the Residual Monitors dialog box from the Convergence Criterion drop-down list.

Edit...

Figure . : The Residual Monitors Dialog Box Displaying Relative or Absolute Convergence

Four options are available for checking an equation for convergence:

absolute

This is the default. For steady-state cases, absolute and none are the only options available for selection.

The residual (scaled and/or normalized) of an equation at an iteration is compared with a user-specified

value. If the residual is less than the user-specified value, that equation is deemed to have converged

for a time step.

relative

The residual of an equation at an iteration of a time step is compared with the residual at the start of

the time step. If the ratio of the two residuals is less than a user-specified value, that equation is deemed

to have converged for a time step.

relative or absolute

If either the absolute convergence criterion or the relative convergence criterion is met, the equation

is considered converged.

The Relative Criteria can be set when relative or relative or absolute is selected.

none

Convergence checking is disabled.

In many situations, the absolute convergence criterion could be too stringent for transient flows

causing a large number of iterations per time step. For example, the scaling of the continuity equation

is based on the value of the continuity residual in the first five iterations. The scaling factor could be

low if the initial continuity residual is small and therefore the scaled residual could fail to meet the

absolute convergence criterion. With the relative convergence criterion, convergence is checked by

comparing the residual at an iteration of a time step with the residual at the beginning of the time

step and hence this problem is alleviated. The relative or absolute convergence criterion is useful

in situations where the residuals of some of the equations are already very low at the start of a time

step (for example, when a particular variable has reached steady-state), and the order of magnitude

reduction in residuals is not possible. The none option allows you to disable convergence checking

by selecting the option in the Convergence Criterion drop-down list.

Important

relative and relative or absolute convergence criteria are available only with the unsteady

pressure-based solver and unsteady density-based solver.

The text command used to access the convergence criterion is

solve → monitors → residual → criterion-type

When criterion-type is entered, you will have the following choices:

Type

Criterion

absolute

relative

none

For criterion-type  or , the text command relative-conv-criteria will appear under

the residual text menu, where the various relative-conv-criteria can be set.

Important

If the NITA solver is enabled, no convergence criteria are available for selection.

.... Modifying Convergence Criteria

Depending on the Convergence Criterion you choose, ANSYS Fluent will check for convergence. If

convergence is being monitored, the solution will stop automatically when each variable meets its

specified convergence criterion. Convergence checks can only be performed on variables whose re-

siduals are being monitored (variables with the Monitor option enabled).

You can choose whether or not you want to check the convergence for each variable by enabling or

disabling the Check Convergence option for it in the Residual Monitors Dialog Box (p. ). To

modify the convergence criterion for a particular variable, enter a new value in the corresponding

convergence criterion field.

.... Disabling Monitoring

If your problem requires the solution of many equations (for example, turbulence quantities and

multiple species), a plot that includes all residuals may be difficult to read. In such cases, you may

choose to monitor only a subset of the residuals, perhaps those that affect convergence the most.

You can indicate whether or not you want to monitor residuals for each variable by enabling or dis-

abling the relevant check box in the Monitor list of the Residual Monitors Dialog Box (p. ).

.... Plot Parameters

If you choose to plot the residual values (either interactively during the solution or using the Plot

button after calculations are complete), there are several display parameters you can modify.

In the Window field under Options, you can specify the ID of the graphics window in which the plot

will be drawn. When ANSYS Fluent is iterating, the active graphics window is temporarily set to this

window to update the residual plot, and then returned to its previous value. Thus, the residual plot

can be maintained in a separate window that does not interfere with other graphical postprocessing.

You can modify the number of residual history points to be displayed in the plot by changing the

Iterations to Plot entry under Options. If you specify  points, ANSYS Fluent will display the last

history points. Since the  axis is scaled by the minimum and maximum values of all points in the

plot, you can zoom in on the end of the residual history by setting Iterations to Plot to a value

smaller than the number of iterations performed. If, for example, the residuals jumped early in the

calculation when you turned on turbulence, that peak broadens the overall range in residual values,

making the smaller fluctuations later on almost indistinguishable. By setting the value of Iterations

to Plot so that the plot does not include that early peak, your -axis range is better suited to the

values that you are interested in seeing. For more information on residual history points, refer to the

discussion of storing residual history points, described earlier in this section.

You can also modify the attributes of the plot axes and the residual curves. Click the Axes... or

Curves... button to open the Axes Dialog Box (p. ) or Curves Dialog Box (p. ). See Axes Dialog

Box (p. ) and Curves Dialog Box (p. ) for details.

Important

Note that entering a value for Iterations to Plot does not necessarily mean solved iterations

but rather stored (or sampled) data points. Note also that the frequency of the data storage

will diminish towards the start of the solution as the number of solved iterations increases.

Due to this, whenever the stored iterations is greater than the solved iterations, if you plot

n iterations, you actually see a history that goes back further than n solved iterations.

.... Postprocessing Residual Values

If you are having solution convergence difficulties, it is often useful to plot the residual value fields

(for example, using contour plots) to determine where the high residual values are located. When

you use the density-based solver, the residual values for all solution variables are available in the

Residuals... category in the postprocessing dialog boxes. (If you read case and data files into ANSYS

Fluent, you will need to perform at least one iteration before the residual values are available for

postprocessing.) For the pressure-based solver, however, only the mass imbalance in each cell is

available by default.

Important

Important

The residual values that are made available for postprocessing are the unscaled values.

If you want to plot residual value fields for a pressure-based solver calculation, you will need to do

. Read in the case and data files of interest (if they are not already in the current session).

. Use the expert command in the solve/set/ text menu to enable the saving of residual values.

Among other questions, ANSYS Fluent will ask if you want to save cell residuals for postprocessing.

Enter yes or y, and keep the default settings for all of the other questions (by pressing the

<RETURN> key).

. Perform at least one iteration.

The solution variables for which residual values are available will appear in the Residuals... category

in the postprocessing dialog boxes. Note that residual values are not available for the radiative

transport equations solved by the discrete ordinates radiation model.

If you are solving a fully-developed periodic flow, you may want to monitor the pressure gradient or

the bulk temperature ratio, as discussed in Periodic Flows (p. ).

If you are solving an unsteady flow (especially if you are using the explicit time stepping option), you

may want to monitor the “time” that has elapsed during the calculation. The physical time of the flow

field starts at zero when you initialize the flow. (See Performing Time-Dependent Calculations (p. )

for details about modeling unsteady flows.)

If you are using an adaptive time stepping method (described in User Inputs for Time-Dependent

Problems (p. )), you may want to monitor the size of the time step,

.

You can create report files and plots for each of these quantities: flow-time, delta-time, iterations-per-

timestep, periodic-pressure-gradient, and periodic-bulk-temperature-ratio. All can be included in a

single report file; flow-time and delta-time can be included in the same report plot, as can periodic-

pressure-gradient and periodic-bulk-temperature-ratio.

For information on setting up report files and plots, see Report Files and Report Plots (p. ).

Solution → Monitors → Report File

New...

Figure . : Report File for 'flow-time', 'delta-time', and 'iters-per-timestep'

Solution quantities for which Report Definitions have been created can be monitored throughout the

solution to aid in judging convergence. You can setup your case file so that force and moment coeffi-

cients and surface and volume integrals are computed and stored at the end of every iteration (for

steady-state solutions) or time step (for transient solutions), and thereby create a convergence history.

You can also choose to compute the value averaged over several iterations/time steps. Running averages

can also help you determine if you have reached convergence for a solution that is oscillating or irreg-

ular. You can print and plot and save this convergence data to an external file using Report Files and

Report Plots. The external file is written in the report file format described in Report Files and Report

Plots (p. ).

Report Files and Report Plots are accessible under the Monitors node in the tree.

Solution → Monitors → Report Files or Report Plots

For additional information on setting up report definitions and report files and plots, see Monitoring

and Reporting Solution Data (p. ) and Creating Report Definitions (p. ).

The convergence conditions facility allows you to set convergence conditions on the solution that are

based on the values from report definitions (surface, volume, lift, drag, and so on). There are two choices

that you must make for declaring convergence using report definitions:

Do you want to check for convergence at every iteration or at every timestep? Make your choice in the

Check For group box.

– Solution Convergence

Fluent checks for solution convergence at every time step.

– Time Step Convergence

Fluent checks for solution convergence at every iteration.

Do you consider the solution converged if all of the active report definitions' criteria and enabled residuals

are satisfied or any of the active report definitions' criteria or enabled residuals is satisfied? Make your choice

in the Choose Condition group box.

– All Conditions are Met

The solution is considered converged when all of the active report definitions' criteria and enabled

residuals are satisfied.

– Any Condition is Met

The solution is considered converged when any of the active report definitions criteria and enabled

residuals is satisfied.

By default, the solution convergence will happen if either report definition convergence criteria or re-

siduals convergence criteria is satisfied. If you want to rely only on the report definition values to decide

convergence, clear the Check Convergence check boxes in the Residual Monitors dialog box.

To open the Convergence Conditions dialog box, click the Convergence... button in the Solution

ribbon tab (Reports group box).

Solution → Reports → Convergence...

Convergence Conditions

The Active column of check boxes (on the left) allows you to deactivate/activate convergence conditions.

... Setting Up the Convergence Conditions Dialog Box

Create new convergence conditions by clicking Add and selecting a Report Definition from the drop-

down list.

To create meaningful conditions for determining convergence from report definitions, set the levels

of the convergence condition variables according to the following directions.

Enter a value in the Ignore Iterations Before | Ignore Time Steps Before column if you expect your

solution to fluctuate in the first few iterations/time steps. Enter a value that represents the number of

iterations/time steps you anticipate the fluctuations to continue. The calculation will begin after this

number of iterations/time steps has finished.

Use the Use Iterations | Use Time Steps setting to select the number of previous iterations/time steps

to be included in the monitor convergence check. For fluctuating simulations like Figure . : Fluctu-

ating Simulation Example (p. ), this number should be high enough to counteract the effect of the

fluctuations.

Figure . : Fluctuating Simulation Example

The Stop Criterion indicates the criterion below which the solution is considered to be converged.

The value of Stop Criterion is calculated as follows:

Res-m() = [abs (m(n) - m(n-))]/m(n)

.

.

.

Res-m(Np) = [abs (m(n) - m(n-Np))]/m(n)

Where:

Res-m is the report definition residual

n is the iteration/time step number

m(n) is the value of the report definition at the nth iteration/time step

Np is the number of previous iterations/time steps to consider (Use Iterations/Use Time Steps)

The report definition residual is the absolute variance of the monitored quantity over the last Np iter-

ations/time steps, divided by the current value of the monitored quantity.

If the maximum value of all of the Res-m values is less than the Stop Criterion number, the solution

is considered to be converged at the nth iteration/time step. If the maximum value of all of the Res-m

values is greater than or equal to the Stop Criterion number, the calculation will proceed to the next

iteration/time step.

Select the Print check box to print report definition residuals in the ANSYS Fluent console. These re-

siduals are calculated as follows with respect to their immediate previous value only.

Pres-m(n) = [abs (m(n) - m(n-))]/m(n)

Where:

Pres- m(n) is the printed residual value for a report definition

n is the iteration that is currently printed in the console

m(n) is the value of the monitor at the nth iteration/time step

Therefore:

Pres-m(n +) = [abs (m(n+) - m(n))]/m(n+)

The printed value at the (n+)th iteration/time step is calculated with respect to the (n)th iteration/time

step and the printed value at the (n)th iteration/time step is calculated with respect to the (n-)th iter-

ation/time step.

As described in Monitoring Solution Convergence (p. ) and Animating the Solution (p. ), respectively,

you can report and monitor various quantities (for example, residuals, force coefficients) and create

animations of the solution while the solver is performing calculations. ANSYS Fluent also includes a

feature that allows you to define your own command(s) to be executed during the calculation at specified

intervals. For example, you can ask ANSYS Fluent to adapt the mesh based on gradient field value cell

registers after a set number of iterations. You will specify a series of text commands or use the GUI to

define the steps to be performed.

Important

Note that the Calculation Activities task page provides options to perform the following

during the calculation:

save case and data files

export transient solution files

export transient particle history data files

Each of these options has their own dialog box, which should be used rather than executing

a command to perform them. See Automatic Saving of Case and Data Files (p. ) and Ex-

porting Data During a Transient Calculation (p. ) for details.

You will indicate the command(s) that you want the solver to execute at specified intervals during the

calculation using the Execute Commands Dialog Box (p. ) (Figure . : The Execute Commands

New...

New...

. Increase the Defined Commands value to the number of commands you want to specify. As this value is

increased, additional command entries will become editable. For each command, you will perform the

. Enable the Active check button next to the command if you want it to be executed during the calculation.

You may define multiple commands and choose to use only a subset of them by turning off the check

button for those that you do not want to use.

. Enter a name for the command under the Name heading.

. Indicate how often you want the command to be executed by setting the interval under Every and selecting

Iteration Time Step or Flow Time in the drop-down list below When. (Time Step and Flow Time are only

valid choices if you are calculating unsteady flow.) For example, to execute the command every  iterations,

you would enter  under Every and select Iteration under When.

Important

If you specify an interval in iterations, be sure to keep the Reporting Interval in the Run

Calculation Task Page (p. ) at its default value of .

Executing Commands During the Calculation

. Define the command by entering a series of text commands in the Command field, or by entering the

name of a command macro you have defined (or will define) as described in Defining Macros (p. ).

Note

Make sure that the text commands you have entered in the Command field of the Execute

Commands dialog box does not exceed  characters.

Important

Note

Important

If the command to be executed involves saving a file, see Saving Files During the Calcula-

tion (p. ) for important information.

If the command enables or disables equations, you must disable the convergence check for

these equations.

... Defining Macros

... Saving Files During the Calculation

You can also use the macros that you define for automatic execution during the calculation, interactively

during the problem setup or postprocessing. For example, if you define a macro that adapts the mesh

after each iteration, you can also use the macro to perform this adaption interactively.

Definition of a macro is accomplished as follows:

. In the Execute Commands Dialog Box (p. ), click the Define Macro... button to open the Define Macro

Dialog Box (p. ) (Figure . :The Define Macro Dialog Box (p. )). Since this is a “modal” dialog box,

the solver will not allow you to do anything else until you perform step , below.

Figure . : The Define Macro Dialog Box

. In the Define Macro dialog box, specify a Name for the macro (for example, adapt1) and click OK. (The

Define Macro... button in the Execute Commands dialog box will become the End Macro button.)

. Perform the steps that you want the macro to perform. For example, if you want the macro to perform

adaption, open the Adaption Controls dialog box, specify the appropriate coarsening, refinement, and

other parameters, and click Adapt to perform the adaption.

Important

Important

. When you have completed the steps you want the macro to perform, click the End Macro button in the

Execute Commands dialog box.

As noted above, once you have defined a macro for execution during the calculation, you can use it

at any time. If you defined the macro called adapt1 to adapt based on pressure gradient, you can

simply type adapt1 in the console to perform this adaption. This macro is independent of any text

menus, so you need not move to a different text menu to use it. Macros can be saved to and read

from files. To save all macros that are currently defined, use the file/write-macros text command.

To read all the macros in a macro file, use the file/read-macros text command.

Important

A macro, like a journal file, is a simple record/playback function. It will therefore know

nothing about the state in which it was recorded or the state in which it is being played

back. You must be careful not to change directories while defining a macro. Also, you must

be careful that all surfaces, variables, and so on that are used by the macro have been

properly defined when you (or ANSYS Fluent) invoke the macro.

If the command to be executed during the calculation involves saving a file, you should include a

special character in the file name when you enter it in The Select File Dialog Box (p. ) so that the

solver will know to assign a new name to each file it saves. See Automatic Numbering of Files (p. )

for details about these special characters for filenames.

Important

Each of these options has their own dialog box, which should be used rather than the Ex-

ecute Commands dialog box. See Automatic Saving of Case and Data Files (p. ) and Ex-

While running a case manually, you can perform certain activities that may facilitate convergence. These

actions may take place before initialization, after initialization and/or at other points during the calcula-

tion. The process described in this section allows you to enter text commands at each of these times

when a case is run from the Run Calculation task page, Workbench, or in batch. In the Calculation

Activities task page, enable Automatically Initialize Solution and Modify Case to automatically

modify the case.

Solution →

Calculation Activities →

Automatically Initialize Solution and Modify Case

→ Edit...

Figure . : The Automatically Initialize Solution and Modify Case Option

When using this option, you can edit the calculation settings. Note that the original settings always

exist and cannot be deleted. The duration of the calculation is defined, so immediately after enabling

Automatically Initialize Solution and Modify Case, you will notice that the Calculation Activities

task page reports that the case will be run with the original settings for a single iteration.

Automatic Initialization of the Solution and Case Modification

You can now control the number of iterations or time steps for the calculation. When Automatically

Initialize Solution and Modify Case option is disabled, you will have to specify the iterations or time

steps using the Run Calculation task page.

For an uninitialized case, clicking the Edit... button will display the Automatic Solution Initialization

and Case Modification dialog box, which allows you to specify the initialization method and to modify

the case.

Figure . : The Automatic Solution Initialization and Case Modification Dialog Box

In the Initialization Method tab, you can specify four different initialization methods:

Initialize with Values from the Case

uses the values set in the Solution Initialization task page.

Note

Hybrid initialization is not performed for this option; even if you have selected Hybrid

Initialization under the Solution Initialization task page.

Use Solution Data from File

requires you to read in a data file containing the desired initialization for this case, as shown in Fig-

ure . :The Automatic Solution Initialization and Case Modification Dialog Box (p. ).

Use Existing Solution Data

is analogous to changing the values in a case and continuing the calculation. However, the iteration counter

will be reset to  so that the modifications can be applied. Use this method when no solution data exists,

similar to the first run.

Important

Whenever the case is initialized, the iteration count is set to .

Important

In the Case Modification tab, you can indicate how long you would like to run with the original settings,

then make any modifications to the case settings.

Figure . : The Case Modification Tab

If you decide to make no modifications, then the counter in the Defined Modifications box will be set

to . However, you still have the option to specify settings that you would like to apply before initializ-

ation, or you can change your original settings. If Before Initialization is enabled, then you can type

the text commands in the Commands field. If Original Settings is enabled, you can type text commands

in the Commands field, and/or specify the Number of Iterations/Time Steps. When entering more

than one text command in a single Commands field, begin each text command with a /, as shown in

Figure . : The Case Modification Tab (p. ).

Note

Make sure that the text commands you have entered in the Commands field does not

exceed  characters.

Important

Note that some text commands require arguments (for example, numbers, file names, yes/no

responses), which are requested through follow-up prompts in the console. When entering

such text commands in the Commands field of the Case Modification tab, be sure to include

your responses to the prompts. If you do not include these responses, the associated com-

mand will not be executed (unless it is a yes/no question, in which case ANSYS Fluent will

use yes by default).

If you decide to run the calculation further with modifications to your case, increase the number of

Defined Modifications and specify additional commands. The settings shown in Figure . : The Case

Modification Tab (p. ) result in the following actions:

. The default initial values for initialization are computed from the velocity-inlet zone Velocity-inlet-.

. The iteration count is set to  (in all situations) and the solution is initialized.

. The calculation is run for  iterations or until convergence.

. The Courant number is set to ..

. The calculation continues for  iterations or until convergence.

. The discretization scheme for turbulent kinetic energy is set to second order upwind, and the Courant

number is set to ..

You can make the above changes sequentially and run your case, or you can specify them all at once.

When you have completed making the modifications, click OK. A Question dialog box may appear,

prompting you to take specific actions. For example, if the Original Settings field is empty, then you

may be notified that the original settings will be lost if the case is saved after the modifications are

applied. It will prompt you for a response when asked if you would like to add commands that specify

the original settings.

Important

If you specify commands for the Original Settings, they will be applied to the case before

the first iteration/time step.

Your actions will be summarized in the Calculation Activities task page, as shown in Figure . : The

Automatically Initialize Solution and Modify Case Option (p. ).

If you disable Automatically Initialize Solution and Modify Case, the settings will be disabled and

retained, but will not be applied to the case.

When Automatically Initialize the Solution and Modify the Case is enabled, settings defined in the

Run Calculation task page will be ignored. Instead, the Number of Iterations will be defined as

Automatic, as shown in Figure . : The Run Calculation Task Page (p. ).

... Altering the Solution Initialization and Case Modification after Calculating

... Altering the Solution Initialization and Case Modification after Cal-

culating

If you decide to edit the solution initialization and case modification settings and one or more iterations

have been calculated, then clicking the Edit... button for the Automatically Initialize Solution and

Modify Case option will open the Edit Automatic Initialization and Case Modifications dialog box,

as shown in Figure . : The Edit Automatic Initialization and Case Modifications Dialog Box (p. ).

Figure . : The Edit Automatic Initialization and Case Modifications Dialog Box

If you select the first option, the initialization controls and modifications that have already taken place

are disabled, therefore you can edit the case modifications that have yet to take place.

If you select the second option, all controls in the Automatic Solution Initialization and Case

Modification dialog box are enabled and therefore, you can modify any of the settings.

During the calculation, you can have Fluent create an animation of mesh (primarily for dynamic mesh

cases), contours, vectors, pathlines, particle tracks, scenes, XY plots, report plots, or residuals. Before

you begin the calculation, you will specify and display the variables and types of plots you want to

animate, and how often you want plots to be saved. At the specified intervals, Fluent will display the

requested plots, and store each one. When the calculation is complete, you can play back the animation

sequence, modify the view (for mesh, contour, vector, pathline, and particle tracks plots), if desired, and

save the animation to a series of picture files or an MPEG file.

Instructions for defining a solution animation sequence are provided in Creating an Animation Defini-

tion (p. ). Playing an Animation Sequence (p. ) describes how to play back and save the animations.

... Creating an Animation Definition

... Playing an Animation Sequence

... Saving an Animation Sequence

... Reading an Animation Sequence

You can use Figure . : The Animation Definition Dialog Box (p. ) to specify the animation object

and the frequency that it will be captured for animating.

Solution → Activities → Create → Solution Animations...

Figure . : The Animation Definition Dialog Box

. (Optional) Enter a Name for the animation definition.

. Indicate how often you want to create a new frame in the animation by specifying a frequency in Record

after every and selecting Iteration, Time Step, or Flow Time.

. Specify how you want Fluent to save the animation frames by selecting In Memory, PPM Image (2D image

file), or HSF File (3D image file) from the Storage Type drop-down.

Important

Viewer” application on iOS and Android equipped devices. The “HOOPS Viewer” applic-

ation can be downloaded to iOS and Android equipped devices from the “App Store”

and “Google Play” respectively.

Animating the Solution

An advantage to saving the animation sequence using the PPM Image option is that

you can use the separate pixmap image files for the creation of a single GIF file. GIF file

creation can be done quickly with graphics tools provided by other third-party graphics

packages such as ImageMagick, that is, animate or convert. For example, if you save

the PPM files starting with the string sequence-, and you are using the ImageMa-

gick software, you can use the convert command with the -adjoin option to create

a single GIF file out of the sequence using the following command.

. Choose the Storage Directory where Fluent save the animation frames.

. (Optional) Specify the graphics Window ID where the animation frames will be displayed during the cal-

culation.

culation.

. (Optional) Specify the Animation View, which determines the orientation of the object for the animation

frames captured during the calculation.

You can only specify the view once an Animation Object is selected. Clicking Preview displays the

selected object in the graphics window specified by Window ID, with the view shown in the drop-

down. If your desired view is not available in the drop-down, you can preview the object, change

its orientation in the graphics window, then click Use Active to save the current graphics window

view and use it for this animation definition.

. Select the graphics object you want to animate from the Animation Object list. If you want to animate

an object that is not listed, you can create a New Object.

Mesh... opens the Mesh Display Dialog Box (p. ).

Contours... opens the Contours Dialog Box (p. ).

Vectors... opens the Vectors Dialog Box (p. ).

Pathlines... opens the Pathlines Dialog Box (p. ).

Particle Tracks... opens the Particle Tracks Dialog Box (p. ).

Scene... opens Figure . :The Scene Dialog Box (p. ).

XY Plot... opens the Solution XY Plot Dialog Box (p. ).

Report Plot... opens the New Report Plot Dialog Box (p. ).

Note

If you select residuals, ensure that Plot is enabled in the Residual Monitors dialog box.

. Click OK to create the animation definition.

.... Guidelines for Creating an Animation Definition

If you are defining an animation sequence containing mesh, contour, or vector displays, note the

following when you are defining the display:

If you want to include lighting effects in the animation frames, be sure to define the lights before you

begin the calculation. See Adding Lights (p. ) for information about adding lights to the display.

If you want to maintain a constant range of colors in a contour or vector display, you can specify a range

explicitly by turning off the Auto Range option in the Contours or Vectors dialog box. See Specifying

the Range of Magnitudes Displayed (p. ) or Specifying the Range of Magnitudes Displayed (p. ) for

details.

Advanced scene manipulations that are specified using the Scene Description dialog box will not be in-

cluded in the animation sequence frames.View modifications such as mirroring across a symmetry plan

will be included.

Once you have defined a sequence (as described in Creating an Animation Definition (p. )) and

performed a calculation, or read in a previously created animation sequence (as described in Reading

an Animation Sequence (p. )), you can play back the sequence using the Playback Dialog Box (p. )

(Figure . : The Playback Dialog Box (p. )).

Results → Animations → Solution Animation Playback

Edit...

Figure . : The Playback Dialog Box

Select the animation you want to play in the Animation Sequences list. To play the animation once

through from start to finish, click the “play” button under the Playback heading. (The buttons function

in a way similar to those on a standard video player.“Play” is the second button from the right—a

single triangle pointing to the right.) To play the animation backwards once, click the “play reverse”

button (the second from the left—a single triangle point to the left). As the animation plays, the Frame

scale shows the number of the frame that is currently displayed, as well as its relative position in the

entire animation. If, instead of playing the complete animation sequence, you want to jump to a par-

ticular frame, move the Frame slider bar to the desired frame number, and the frame corresponding

to the new frame number will be displayed in the graphics window.

Important

For smoother animations, enable the Double Buffering option in the Display Options Dialog

Box (p. ) (see Modifying the Rendering Options (p. )). This will reduce screen flicker

during graphics updates.

Note

For HSF File and In Memory 3D animations, you can disable Use Stored View to manipulate

the view during playback.

Additional options for playing back animations are described below.

.... Modifying the View

If you want to replay the animation sequence with a different view of the scene, you can use your

mouse to modify (for example, translate, rotate, zoom) it in the graphics window where the animation

is displayed. Note that any changes you make to the view for an animation sequence will be lost

when you select a new sequence (or reselect the current sequence) in the Sequences list.

.... Modifying the Playback Speed

Different computers will play the animation sequence at different speeds, depending on the complexity

of the scene and the type of hardware used for graphics. You may want to slow down the playback

speed for optimal viewing. Move the Replay Speed slider bar to the left to reduce the playback speed

(and to the right to increase it).

.... Playing Back an Excerpt

You may sometimes want to play only one portion of a long animation sequence. To do this, you can

modify the Start Frame and the End Frame under the Playback heading. For example, if your anim-

ation contains  frames, but you want to play only frames  to , you can set Start Frame to

and End Frame to . When you play the animation, it will start at frame  and finish at frame .

....“Fast-Forwarding” the Animation

You can “fast-forward” or “fast-reverse” the animation by skipping some of the frames during playback.

To fast-forward the animation, you will need to set the Increment and click the fast-forward button

(the last button on the right—two triangles pointing to the right). If, for example, your Start Frame

is , your End Frame is , and your Increment is , when you click the fast-forward button, the an-

imation will show frames , , , , , ,  and . Clicking on the fast-reverse button (the first

button on the left—two triangles pointing to the left) will show frames , , ,....

.... Continuous Animation

If you want the playback of the animation to repeat continuously, there are two options available.

To continuously play the animation from beginning to end (or from end to beginning, if you use one

of the reverse play buttons), select Auto Repeat in the Playback Mode drop-down list. To play the

animation back and forth continuously, reversing the playback direction each time, select Auto Reverse

in the Playback Mode drop-down list.

To turn off the continuous playback, select Play Once in the Playback Mode list. This is the default

setting.

.... Stopping the Animation

To stop the animation during playback, click the “stop” button (the square in the middle of the

playback control buttons). If your animation contains very complicated scenes, there may be a slight

delay before the animation stops.

.... Advancing the Animation Frame by Frame

To advance the animation manually frame by frame, use the third button from the right (a vertical

bar with a triangle pointing to the right). Each time you click this button, the next frame will be dis-

played in the graphics window. To reverse the animation frame by frame, use the third button from

the left (a left-pointing triangle with a vertical bar). Frame-by-frame playback allows you to freeze the

animation at points that are of particular interest.

.... Deleting an Animation Sequence

If you want to remove one of the sequences that you have created or read in, select it in the Sequences

list and click the Delete button. If you want to delete all sequences, click the Delete All button.

Important

Note that if you delete a sequence that has not yet been saved to disk (that is, if you se-

lected In Memory under Storage Type in the Animation Sequence dialog box), it will

be removed from memory permanently. If you want to keep any animation sequences that

are stored only in memory, you should be sure to save them (as described in Saving an

Animation Sequence (p. )) before you delete them from the Sequences list or exit ANSYS

Fluent.

Once you have created an animation sequence, you can save it in any of the following formats:

Solution animation file containing the ANSYS Fluent metafiles

Picture files, each containing a frame of the animation sequence

MPEG file containing each frame of the animation sequence

Note that, if you are saving picture files or an MPEG file, you can modify the view (for example, translate,

rotate, zoom) in the graphics window where the animation is displayed, and save the modified view

instead of the original view.

.... Solution Animation File

If you selected HSF File or PPM Image for Storage Type in Figure . : The Animation Definition

Dialog Box (p. ), then Fluent will save the solution animation file for you automatically. It will be

saved in the specified Storage Directory, and its name will be the Name you specified for the se-

quence, with a .cxa extension (for example, pressure-contour.cxa). In addition to the .cxa

file, Fluent will also save image files with .hsf or .ppm extensions for each frame (for example,

pressure-contour_0002.hsf). The .cxa file contains a list of the associated .hsf or .ppm

files, and tells Fluent the order in which to display them.

If you selected In Memory under Storage Type, then the solution animation file (.cxa) and the as-

sociated files (.hmf) will be lost when you exit from ANSYS Fluent, unless you save them as described

below.

You can save the animation sequence to a file that can be read back into ANSYS Fluent (see Reading

an Animation Sequence (p. )) when you want to replay the animation. As noted in Reading an

Animation Sequence (p. ), the solution animation file can be used for playback in Fluent independent

of the case and data files that were used to generate it.

To save a solution animation file (and the associated files), select Animation Frames in the

Write/Record Format drop-down list in the Playback dialog box, and click the Write button. ANSYS

Fluent will save a .cxa file, as well as a .hmf file for each frame of the animation sequence. The fi-

lename for the .cxa file will be the specified sequence Name (for example, pressure-con-

tour.cxa), and the file names for the metafiles will consist of the specified sequence Name followed

by a frame number (for example, pressure-contour_0002.hmf). All of the files (.cxa and .hmf)

will be saved in the current working directory.

.... Picture File

You can also generate a picture file for each frame in the animation sequence. This feature allows

you to save your sequence frames to picture files used by an external animation program such as

ImageMagick. As noted above, you can modify the view in the graphics window before you save the

picture files.

To save the animation as a series of picture files, follow these steps:

. Select Picture Files in the Write/Record Format drop-down list in the Playback dialog box.

. If necessary, click the Picture Options... button to open the Save Picture Dialog Box (p. ) and set the

appropriate parameters for saving the picture files. (If you are saving picture files for use with ImageMagick,

for example, you may want to select the window dump format. See Window Dumps (Linux Systems

Only) (p. ) Apply in the Save Picture dialog box to save your modified settings.

Important

Do not click the Save... button in the Save Picture dialog box.You will save the picture

files from the Playback dialog box in the next step.

The AVZ and VRML formats are not supported for writing solution animation picture files.

. In the Playback dialog box, click the Write button. ANSYS Fluent will replay the animation, saving each

frame to a separate file.The filenames will consist of the specified sequence Name followed by an anim-

ation sequence and a frame number (for example, pressure-contour_1_0002.ps), and they will

all be saved in the current working directory.

.... MPEG File

It is also possible to save all of the frames of the animation sequence in an MPEG file, which can be

viewed using an MPEG decoder such as mpeg_play. Saving the entire animation to an MPEG file will

require less disk space than storing individual window dump files (using the picture method), but

the MPEG file will yield lower-quality images.

As noted above, you can modify the view in the graphics window before you save the MPEG file.

To save the animation to an MPEG file, follow these steps:

. Select MPEG in the Write/Record Format drop-down list in the Playback dialog box.

. Click the Write button.

ANSYS Fluent will replay the animation and save each frame to a separate scratch file, and then

it will combine all the files into a single MPEG file. The name of the MPEG file will be the specified

sequence Name with an .mpg extension (for example, pressure-contour.mpg), and it will

be saved in the current working directory.

If you have saved an animation sequence to a solution animation file (as described in Saving an Anim-

ation Sequence (p. )), you can read that file back in at a later time (or in a different session) and

play the animation. Note that you can read a solution animation file into any ANSYS Fluent session;

you do not need to read in the corresponding case and data files. In fact, you do not need to read in

any case and data files at all before you read a solution animation file into ANSYS Fluent.

To read a solution animation file, click the Read... button in the Playback Dialog Box (p. ). In The

Select File Dialog Box (p. ), specify the name of the file to be read.

After you have set up your case, and prior to solving it, you can check your case setup using the Case

Check Dialog Box (p. ) (Figure . : The Case Check Dialog Box (p. )). This function provides you

with guidance and best practices when choosing case parameters and models. Your case will be checked

for compliance in the mesh, models, boundary and cell zone conditions, material properties, and solver

categories. Established rules will be available for each category, with recommended changes to your

current settings. At your discretion, you may elect to apply the recommendations, or keep your current

settings.

To access the Case Check Dialog Box (p. ) (Figure . : The Case Check Dialog Box (p. )), go to

Checking Your Case Setup

Check Case...

If there are no problems with your case setup, then an information dialog box (Figure . : The Inform-

ation Dialog Box (p. )) will appear stating that no recommendations need to be made at this time,

otherwise, the Case Check Dialog Box (p. ) will open.

Figure . : The Case Check Dialog Box

Figure . : The Information Dialog Box

In the Case Check dialog box, each of the tabs Mesh, Models, Boundaries and Cell Zones, Materials,

and Solver may contain recommendations. For each of the tabs that are enabled, best practices will

be listed.

In some cases, the dialog box will be split based on the method that the recommendation is applied.

There are two ways you can apply the listed recommendations:

Automatic Implementation

ANSYS Fluent applies the change for you.

Manual Implementation

You will manually change your case settings.

... Automatic Implementation

... Manual Implementation

To the left of each of the recommendations listed under Automatic Implementation (for example,

Figure . : The Models Tab in the Case Check Dialog Box (p. )), there is an enabled Apply check

box. An enabled check box will result in ANSYS Fluent applying the change to your case automatically.

If there are some recommendations that you do not want ANSYS Fluent to implement automatically,

then click the Apply check box to toggle off and disable the implementation of a particular recom-

mendation. After going through all the tabs and determining which rules you want applied automat-

ically, click the Apply button at the bottom of the dialog box. Changes to your settings will be applied

to all recommendations throughout the dialog box with an enabled Apply check box. ANSYS Fluent will

print a message in the console notifying you that the applied recommendation has been implemented.

ANSYS Fluent will ask you if you want to save the case before proceeding to the next step. If you

choose Yes, The Select File Dialog Box (p. ) will open allowing you to save your case with the new

settings. If you select No, all the changes made to the case file will be lost once you exit ANSYS Fluent.

For recommendations that are listed under Manual Implementation, ANSYS Fluent cannot apply the

changes for you. Therefore, if you opt to make a change to your current settings, based on the listed

recommendations, then you will need to manually make the changes by opening the affected dialog

boxes or task pages and applying what was recommended.

To the right of the recommendations is a ?, which essentially acts as a help button, leading you to

related documentation on the specific topic.

At the bottom of each recommendation, there is a path that will guide you to the dialog box or task

page where you can make the changes. For example, in the Mesh tab, you will see the following re-

commendation:

Check your mesh.

(General: Click [Check])

To perform the action, highlight General in the tree, then click the Check button in the Mesh group

box. You will see a path for each recommendation, in each of the tabs.

Each of the case check rules are described in the following sections:

.... Checking the Mesh

.... Checking Model Selections

.... Checking Boundary and Cell Zone Conditions

.... Checking Material Properties

.... Checking the Solver Settings

Figure . : The Mesh Tab in the Case Check Dialog Box

The following recommendations appear under the Mesh tab (Figure . : The Mesh Tab in the Case

Check Dialog Box (p. )):

If you have not already checked your mesh, it is best practice that you do so immediately after

reading in your mesh, or after any mesh modification. To check your mesh go to

Setup →

Checking the mesh will help you detect any mesh trouble before you get started with your problem

setup. You can learn more about the information obtained when checking your mesh, by going to

Checking the Mesh (p. ).

Improve the mesh quality before proceeding with your simulation.The maximum cell skewness is

greater than ..

Check the quality of your mesh immediately after reading in your mesh, or after any mesh modific-

ation. The quality of the mesh plays a significant role in the accuracy and stability of the numerical

computation. You can learn more about the quality of your mesh by going to Mesh Quality (p. ).

Setup →

Preview zone motion and mesh motion before beginning the simulation.

Setup →

After setting up your case using the Dynamic Mesh model, it is worth while to preview your mesh

prior to running your simulation. You can preview Zone Motion by going to

Setup →

To preview the Mesh Motion, go to

Setup →

or

or

Solution →

Run Calculation → Preview Mesh Motion...

It is important that you preview zone motion first and then mesh motion. Zone motion shows the

motion of all dynamic zones with the prescribed rigid body motion, using the graphics library. It

is a very fast process and does not alter the mesh. Previewing the zone motion will show you if

the motion is set up properly (for example zones moving in the wrong direction or rotating about

the wrong center). It is much more difficult to detect these problems with mesh motion because

small time steps are performed and no continuous animation is shown.

Mesh motion should always be done for dynamic mesh cases with prescribed motion. Mesh motion

will only show the validity of the mesh during the simulation. Mesh deformation and dynamic

zones without rigid body motion will be considered during a mesh motion preview.

Both the Mesh Motion and Zone Motion dialog boxes will have a Preview button that will allow

you to view the mesh or zone motion prior to running your case. You can obtain more information

on mesh motion and zone motion by going to Previewing the Dynamic Mesh (p. ).

Translate the mesh for axisymmetric geometry containing nodes below the x-axis.

If either Axisymmetric or Axisymmetric Swirl is specified in the General task page and there are

mesh nodes that fall below the x-axis, then it is recommended that you translate the mesh. Nodes

below the  axis are forbidden for axisymmetric cases, since the axisymmetric cell volumes are

created by rotating the 2D cell volume about the  axis; therefore nodes below the  axis would

create negative volumes. To find out if there are any nodes that lie below the x-axis, perform a

mesh check (Checking the Mesh (p. )). For information on translating the mesh, see Translating

the Mesh (p. ). To access the Mesh Translate dialog box, go to

Figure . : The Models Tab in the Case Check Dialog Box

The following recommendations appear under the Models tab (Figure . : The Models Tab in the

Case Check Dialog Box (p. )):

Consider realizable k-epsilon in lieu of the standard k-epsilon turbulence model.

The realizable -  model is a more recent development of the standard -  model and differs

from it in that the realizable -  model contains a new formulation for the turbulent viscosity, as

well as a new transport equation for the dissipation rate, , derived from an exact equation for the

transport of the mean-square vorticity fluctuation.

realizable -  model means that the model satisfies certain mathematical constraints on the

Reynolds stresses, consistent with the physics of turbulent flows. For more information on the

standard -  model and the realizable -  model, visit Standard k-ε Model and Realizable k-

ε Model (in the Theory Guide), respectively.

Setup →

Models →

For information on all -  model options, go to Standard, RNG, and Realizable k-ε Models in the

Disable DO/Energy coupling if the optical thickness is less than .

DO/Energy coupling should only be used when the optical thickness is greater than . Refer to

Energy Coupling and the DO Model in the Theory Guide for more information.

Setup →

Models →

Radiation → Edit...

Verify that the temperature specified for boundary zones that do not participate in the view factor

calculation is appropriate.

When using the S2S radiation model, make sure that you set the temperature for boundaries that

do not participate in the view factor calculation to an appropriate value. In most cases the appro-

priate value is the ambient temperature, which by default is assumed to be  K. See Specifying

Boundary Zone Participation (p. ) for more information.

Setup →

Models →

Change the under-relaxation factor for the mixing plane model to ..

If you have created a mixing plane, set the Under-Relaxation in the Mixing Plane dialog box to

. Look under Global Parameters in Setting Up the Mixing Plane Model (p. ) for information

about the mixing plane under-relaxation.

Enable the smoothing option for dynamic mesh simulations when remeshing.

When your case involves the use of dynamic meshes and remeshing is enabled, then it is recom-

mended that you also perform smoothing on the mesh. For a complete discussion of smoothing

and remeshing, see Setting Dynamic Mesh Modeling Parameters (p. ).

Setup →

Disable species inlet diffusion for laminar flow with species transport.

By default, ANSYS Fluent includes the diffusion flux of species at inlets. In some cases involving

species transport and laminar flow, it is recommended that the Inlet Diffusion option in the Species

Model dialog box is disabled. For example,

– If you want to include only the convective transport of species through the inlets of your domain.

– If at one of the inlets, the convective flux is very small, resulting in mass loss by diffusion through the

inlet.

Setup →

Models →

For more information about diffusion at inlets, go to Defining Cell Zone and Boundary Conditions

for Species (p. ).

Include turbulence interaction for the NOx model.

When running thermal NOx simulations and your flow is turbulent, then be sure to set the NOx

Turbulence Interaction Mode.

Setup →

Models →

NOx → Edit...

In turbulent combustion calculations, ANSYS Fluent solves the density-weighted time-averaged

Navier-Stokes equations for temperature, velocity, and species concentrations or mean mixture

fraction and variance. Methods of modeling the mean turbulent reaction rate can be based on

either moment methods or probability density function (PDF) techniques. ANSYS Fluent uses the

PDF approach.

To learn about how this feature is set up, go to Setting Turbulence Parameters (p. ).

Consider using the default Schnerr-Sauer or the Zwart-Gerber-Belamri cavitation model.

When using the mixture multiphase model with the Singhal et al. cavitation model enabled, consider

changing it to either the Schnerr-Sauer or the Zwart-Gerber-Belamri cavitation model. Refer to

Cavitation Models in the Theory Guide for more information.

Setup → Models → Phases → Interaction...

Figure . : The Boundaries and Cell Zones Tab in the Case Check Dialog Box

The following recommendations appear under the Boundaries and Cell Zones tab (Figure . : The

Boundaries and Cell Zones Tab in the Case Check Dialog Box (p. )):

Apply an axis boundary on the centerline (x-axis).

For geometry that is axisymmetric or axisymmetric swirl (as set in the General task page), the

centerline (x-axis) boundary type should be set to axis. See Axis Boundary Conditions (p. ).

Change outlet boundary conditions. A combination of pressure and outflow boundaries is not

compatible.

Outflow boundary conditions in ANSYS Fluent are used to model flow exits where the details of

the flow velocity and pressure are not known prior to solution of the flow problem. One of the

limitations when using outflow boundary conditions is that outflow boundary conditions are not

compatible with pressure inlets. Therefore, it is recommended that you use velocity or mass-flow

inlets instead of pressure inlets when used in combination with outflow boundaries. See Outflow

Boundary Conditions (p. ) for a list of limitations that exist with outflow boundaries.

Setup →

Change outlet boundary conditions. Outflow boundary conditions are not compatible with the

ideal gas law for density.

Setup →

Outflow boundaries cannot be used if you are modeling unsteady flows with varying density, even

if the flow is incompressible. See Outflow Boundary Conditions (p. ) for more limitations that

exist with outflow boundaries.

Setup →

Non-zero operating pressure set.This will be added to gauge pressure inputs.

For cases that have density specified as the ideal gas law, and the operating pressure is greater

than zero, the operating pressure will be added to the gauge pressure to yield the absolute pressure.

For more information, see Density Inputs for the Ideal Gas Law for Compressible Flows (p. ) and

Operating Pressure, Gauge Pressure, and Absolute Pressure (p. ).

Setup →

Apply positive non-zero pressure boundary conditions when using the ideal gas law for density.

In compressible flows , isentropic relations for an ideal gas are applied to relate total pressure,

static pressure, and velocity at a pressure inlet boundary. Your input of total pressure,

, at the

inlet and the static pressure,

, in the adjacent fluid cell are related, as described in Equa-

tion . (p. ) Equation . (p. ) of Calculation Procedure at Pressure Inlet Boundaries (p. ).

It is recommended that pressure boundary conditions are not set to zero for compressible flows

that use the ideal gas law.

Setup →

Review turbulence specifications at flow boundaries. Default values detected.

If your case setup has any of the turbulence models enabled, be sure to review the default para-

meters for K and Epsilon or K and Omega for the Turbulence Specification Method in the outlet

and inlet boundary conditions. ANSYS Fluent’s default parameters for the (Backflow) Turbulent

Kinetic Energy, (Backflow) Turbulent Dissipation Rate, and (Backflow) Specific Dissipation Rate

are . You can either adjust the values, or select a different Turbulence Specification Method.

For general information turbulence parameters, see Determining Turbulence Parameters (p. ).

Setup →

Assign non-zero layer thicknesses for wall boundaries with shell conduction.

When the Shell Conduction option is enabled in the Wall boundary condition dialog box, ANSYS

Fluent will compute heat conduction for the wall not only in the normal direction, but also in the

planar directions. To enable such computations, you must specify a nonzero Thickness for each

layer in the Shell Conduction Layers dialog box. See Shell Conduction (p. ) for information on

shell conduction in thin walls.

Setup →

Assign a value of  or  for VOF at the inlet or outlet boundary conditions.

When enabling the VOF model, the Volume Fraction in the inlet and outlet boundary conditions

for each phase should be set either to  or . No intermediate values are permitted. For general

information on boundary condition setup, see Defining Multiphase Cell Zone and Boundary Condi-

Setup →

Change the outlet boundary condition. Outflow boundary condition is not compatible with current

multiphase settings.

Setup →

You cannot assign an outflow boundary condition when using the mixture and Eulerian multiphase

models. Note the limitations of this boundary condition in Outflow Boundary Conditions (p. ).

ANSYS Fluent can model the effects of open channel flow using the VOF formulation. In such a

case, outflow boundary conditions can be used at the outlet of open channel flows, to model flow

exits where the details of the flow velocity and pressure are not known prior to solving the flow

problem. See Open Channel Flow in the Theory Guide, under the heading Outflow Boundary, for

Setup →

Review wall motion. Stationary wall motion relative to adjacent cell zone detected.

In cases where the fluid zone motion type is specified as Moving Mesh or Moving Reference

Frame, all wall zones should be set to Moving Wall in the Momentum tab in the Wall boundary

conditions dialog box. The wall motion should be defined Relative to Adjacent Cell Zone. The

exception to this is if the walls are stationary in the absolute frame. To define wall motion, see Inputs

at Wall Boundaries (p. ).

Setup →

Assign non-zero velocities when specifying a moving fluid zone.

If selecting either Moving Mesh or Moving Reference Frame in the Fluid dialog box, be sure to

set nonzero values for the rotational and translational velocities. Refer to Defining Zone Mo-

tion (p. ) for user inputs.

Setup →

Review flow specifications at inlet boundaries. Default values detected.

Setup →

For mass-flow-inlet and velocity-inlet boundary conditions, the default values in ANSYS Fluent are

and

, respectively. Review the settings and adjust accordingly. See Default Settings

at Velocity Inlet Boundaries (p. ) and Default Settings at Mass-Flow Inlet Boundaries (p. ) for

default parameters of velocity inlets and mass-flow inlets, respectively.

Setup →

Define the porous zone when using the heat exchanger model.

Heat exchanger models always require the definition of the porous media zone on the primary

side for the macro model and for both primary and auxiliary sides for the dual cell model. See

Streamwise Pressure Drop in the Theory Guide for more information.

Setup →

Figure . : The Materials Tab in the Case Check Dialog Box

The following recommendations appear under the Materials tab (Figure . : The Materials Tab in

the Case Check Dialog Box (p. )):

Assign individual fluid Cps to polynomial functions of temperature.

For cases with species transport and volumetric reactions, it is best practice to specify the specific

as a polynomial that is a function of temperature. See Defining Properties for the

Mixture and Its Constituent Species (p. ) and Specific Heat Capacity as a Function of Temperat-

ure (p. ) for information on defining material properties for the species in the mixture.

Setup →

Materials

Assign a non-zero value for the density when selecting boussinesq.

The Boussinesq model is used for natural convection problems involving small changes in temper-

Setup →

Materials

ature. To enable the Boussinesq approximation for density, choose boussinesq from the Density

drop-down list in the Create/Edit Materials dialog box and specify a constant value for Density.

See Inputs for the Boussinesq Approximation (p. ).

Setup →

Materials

Review the absorption coefficient. Default value detected.

If any of the radiation models are enabled. Enter an absorption coefficient for the material listed

(Radiation Properties (p. )).

Setup →

Materials

Assign a non-zero thermal expansion coefficient when selecting the Boussinesq density model.

When selecting boussinesq to describe the density of your material, be sure to enter a valid thermal

expansion coefficient for your material. For detailed information on the Boussinesq model, see The

Boussinesq Model (p. ).

Setup →

Materials

Figure . : The Solver Tab in the Case Check Dialog Box

The following recommendations appear under the Solver tab (Figure . : The Solver Tab in the

Enable the unsteady solver option when selecting moving mesh for the fluid boundary.

If the motion type of the fluid boundary condition is specified as Moving Mesh, then your case

should be specified as Transient in the General task page. Visit Setting Up the Sliding Mesh

Problem (p. ) for steps on setting up moving mesh problem.

Setup →

General

Assign LSQ cell-based gradient reconstruction.

The least squares cell-based averaging scheme is known to be as accurate as the node-based

Setup →

General

gradient for irregular unstructured meshes, but less expensive to compute than the node-based

gradient. Therefore, it is recommended that least squares cell-based gradient reconstruction is used.

See Evaluation of Gradients and Derivatives in the Theory Guide for more information on gradient

options.

Solution →

Methods

Change the under-relaxation factor for the energy equation to at least ..

You should set the energy under-relaxation factor between . and .. If you decide to apply

this recommendation, then ANSYS Fluent will automatically set the energy under-relaxation factor

to .. If you want to increase this value, you can manually make the change by going to the

Solution Controls task page. See Solution Strategies for Heat Transfer Modeling (p. ) for the

under-relaxation of the energy equation.

Solution →

Controls

Increase the NOx under-relaxation factor to at least ..

If the NOx model is enabled, set the NOx under-relaxation factor to a value of at least . to fully

converge the solution. Note that the under-relaxation factor could be lower at the start of the run,

but can then be increased after an initial solution is obtained. If you decide to apply this recom-

mendation, then ANSYS Fluent will automatically set the NOx under-relaxation factor to .. If

you want to increase this value, you can manually make the change by going to the Solution

Controls task page. See Using the NOx Model (p. ).

Solution →

Controls

Increase the Discrete Ordinates under-relaxation factor to at least ..

Solution →

Controls

If the Discrete Ordinates (DO) radiation model is enabled, set the radiation under-relaxation factor

to a value of at least . to fully converge the solution. Note that the under-relaxation factor could

be lower at the start of the run, but can then be increased after an initial solution is obtained. If

you decide to apply this recommendation, then ANSYS Fluent will automatically set the radiation

under-relaxation factor to .. If you want to increase this value, you can manually make the

change by going to the Solution Controls task page. See DO Solution Parameters (p. ).

Solution →

Controls

Increase the P1 under-relaxation factor to ..

If the P1 radiation model is enabled, set the radiation under-relaxation factor to . to fully converge

the solution. Note that the under-relaxation factor could be lower at the start of the run, but can

then be increased after an initial solution is obtained. If you decide to apply this recommendation,

then ANSYS Fluent will automatically set the radiation under-relaxation factor to .. See P-

Model Solution Parameters (p. ).

Solution →

Controls

Increase the species and energy under-relaxation factors to at least ..

For a case with species transport and energy defined, set the species and energy under-relaxation

factors to a value of at least .. If you decide to apply this recommendation, then ANSYS Fluent will

automatically set the species and energy under-relaxation factors to .. If you want to increase

this value, you can manually make the change by going to the Solution Controls task page. See

Solution Procedures for Chemical Mixing and Finite-Rate Chemistry (p. ).

Solution →

Controls

Assign a value of  for the under-relaxation factor for unsteady DPM with  DPM update per time

step.

It is recommended that the DPM under-relaxation factor be set to  for unsteady DPM with  DPM

update per time step.

Solution →

Controls

Increase the mean mixture fraction under-relaxation factor to at least ..

If the non-premixed or partially premixed combustion models are enabled, then it is best to set

the mean mixture under-relaxation factor to a value of at least . to ensure full convergence. If

you decide to apply this recommendation, then ANSYS Fluent will automatically set the mean

mixture under-relaxation factor to .. If you want to increase this value, you can manually make

the change by going to the Solution Controls task page. See Solving the Flow Problem (p. ).

Solution →

Controls

Consider using higher order discretization for improved accuracy of the final solution. First-order

discretization may be used in the initial solution.

It is generally advisable to obtain an initial solution using first-order accurate discretization, however,

second order discretization is recommended for improved accuracy of the final solution. See

Choosing the Spatial Discretization Scheme (p. ) for more information on discretization schemes.

Solution →

Methods

Select the absolute reference frame for initializing cases when using the MRF model.

When using the MRF model, always use the absolute reference frame while initializing the solution.

Select Absolute under Reference Frame in the Solution Initialization task page. If the Relative

to Cell Zone option is selected, which is the default option, the initial flow field can contain discon-

tinuities, which can cause convergence problems in the first few iterations. Refer to Initializing the

Entire Flow Field Using Standard Initialization (p. ) for more information.

Initialize

Choose PRESTO! for the pressure discretization scheme.

When using the VOF model, it is recommended that you use PRESTO! as the pressure discretization

scheme. This scheme is recommended for flows with high swirl numbers, a high-Rayleigh-number

natural convection, high-speed rotating flows, flows involving porous media, and flows in strongly

curved domains. See Choosing the Pressure Interpolation Scheme (p. ) for more information.

Solution →

Methods

Convergence can be hindered by a number of factors. Large numbers of computational cells, overly

conservative under-relaxation factors, and complex flow physics are often the main causes. Sometimes

it is difficult to know whether you have a converged solution. In the following sections, some of the

numerical controls and modeling techniques that can be exercised to enhance convergence and

maintain stability are examined.

... Judging Convergence

... Step-by-Step Solution Processes

... Modifying Algebraic Multigrid Parameters

... Modifying the Multi-Stage Parameters

... Robustness on Meshes of Poor Quality

...Warped-Face Gradient Correction

You should also refer to Choosing the Spatial Discretization Scheme (p. ) and Choosing the Pressure-

Velocity Coupling Method (p. ) for information about how the choice of discretization scheme or (for

the pressure-based solver) pressure-velocity coupling scheme can affect convergence. Manipulation of

under-relaxation parameters and multigrid settings to enhance convergence is discussed in Setting

Under-Relaxation Factors (p. ) and Modifying Algebraic Multigrid Parameters (p. ).

There are no universal metrics for judging convergence. Residual definitions that are useful for one

class of problem are sometimes misleading for other classes of problems. Therefore it is a good idea

to judge convergence not only by examining residual levels, but also by monitoring relevant integrated

quantities such as drag or heat transfer coefficient.

For many problems, the default convergence criterion in ANSYS Fluent is sufficient. This criterion requires

that the globally scaled residuals, defined by Equation . (p. ) or Equation . (p. ) decrease

to

for all equations except the energy and P- equations, for which the criterion is

.

Sometimes, however, this criterion may not be appropriate. For example:

Because the continuity residual is scaled by its behavior during the first five iterations, the continuity residual

level is initial guess-dependent and startup-dependent. A better initial guess may lead to a higher continuity

residual, which is counter-intuitive for judging convergence.

Because the global scale factors depend on the solution level, sometimes the residuals are significantly

below the default convergence target even when the solution is still changing.This behavior occurs most

frequently with the energy equation.

For some equations, such as for turbulence quantities, a poor initial guess may result in high scale factors.

In such cases, scaled residuals will start low, increase as nonlinear sources build up, and eventually decrease.

It is therefore good practice to judge convergence not just from the value of the residual itself, but from

its behavior.You should ensure that the residual continues to decrease (or remain low) for several iterations

(say  or more) before concluding that the solution has converged.

When issues like the above arise, you should consider using locally scaled residuals defined by Equa-

tion . (p. ) or Equation . (p. ), which have a default convergence criterion of - for all

equations. Experience suggests that locally scaled residuals may be more universal for the purposes

of judging convergence than globally scaled residuals.

Another popular approach to judging convergence is to require that the unscaled residuals drop by

three orders of magnitude. ANSYS Fluent provides residual normalization for this purpose, as discussed

in Definition of Residuals for the Pressure-Based Solver (p. ), where residuals are defined for both

the pressure-based solver and the density-based solver. In this approach the convergence criterion is

that the normalized unscaled residuals should drop to

. However, this requirement may not be

appropriate in many cases:

Convergence and Stability

If you have provided a very good initial guess, the residuals may not drop three orders of magnitude. In a

nearly-isothermal flow, for example, energy residuals may not drop three orders if the initial guess of

temperature is very close to the final solution.

If the governing equation contains nonlinear source terms which are zero at the beginning of the calculation

and build up slowly during computation, the residuals may not drop three orders of magnitude. In the

case of natural convection in an enclosure, for example, initial momentum residuals may be very close to

zero because the initial uniform temperature guess does not generate buoyancy. In such a case, the initial

nearly-zero residual is not a good scale for the residual.

If the variable of interest is nearly zero everywhere, the residuals may not drop three orders of magnitude.

In fully-developed flow in a pipe, for example, the cross-sectional velocities are zero. If these velocities have

been initialized to zero, initial (and final) residuals are both close to zero, and a three-order drop cannot

be expected.

Regardless of the residual scaling method, it is wise to monitor important solution quantities, such as

drag or overall heat transfer coefficient, before concluding that the solution has converged.

Conversely, it is possible that if the initial guess is very bad, the initial residuals are so large that a

three-order drop in residual does not guarantee convergence. This is specially true for  and  equations

where good initial guesses are difficult. Here again it is useful to examine overall integrated quantities

that you are particularly interested in. If the solution is unconverged, you may drop the convergence

tolerance, as described in Modifying Convergence Criteria (p. ).

One important technique for speeding convergence for complex problems is to tackle the problem

one step at a time. When modeling a problem with heat transfer, you can begin with the calculation

of the isothermal flow. To solve turbulent flow, you might start with the calculation of laminar flow.

When modeling a reacting flow, you can begin by computing a partially converged solution to the

non-reacting flow, possibly including the species mixing. When modeling a discrete phase, such as

fuel evaporating from droplets, it is a good idea to solve the gas-phase flow field first. Such solutions

generally serve as a good starting point for the calculation of the more complex problems. These step-

by-step techniques involve using the Solution Controls Task Page (p. ) to turn equations on and off

in the Equations dialog box.

.... Selecting a Subset of the Solution Equations

ANSYS Fluent automatically solves each equation that is turned on using the Models family of dialog

boxes. If you specify in the Viscous Model Dialog Box (p. ) that the flow is turbulent, equations for

conservation of turbulence quantities are turned on. If you specify in the Energy Dialog Box (p. )

that ANSYS Fluent should enable energy, the energy equation is enabled. Convergence can be sped

up by focusing the computational effort on the equations of primary importance. The Equations list

in the Equations Dialog Box (p. ) allows you to turn individual equations on or off temporarily.

A typical example is the computation of a flow with heat transfer. Initially, you will define the full

problem scope, including the thermal boundary conditions and temperature-dependent flow properties.

Following the problem setup, you will use the Equations dialog box to temporarily turn off the energy

equation. You can then compute an isothermal flow field, remembering to set a reasonable initial

value for the temperature of the fluid.

Important

This is possible only for the pressure-based solver; the density-based solver solves the energy

equation together with the flow equations in a coupled manner, so you cannot turn off

the energy equation as described above.

When the isothermal flow is reasonably well converged, you can turn the energy equation back on.

You can actually turn off the momentum and continuity equations while the initial energy field is

being computed. When the energy field begins to converge well, you can turn the momentum and

continuity equations back on so that the flow pattern can adjust to the new temperature field. The

temperature will couple back into the flow solution by its impact on fluid properties such as density

and viscosity. The temperature field will have no effect on the flow field if the fluid properties (for

example, density, viscosity) do not vary with temperature. In such cases, you can compute the energy

field without turning the flow equations back on again.

Important

Important

If you have specified temperature-dependent flow properties, you should be sure that a

realistic value has been set for temperature throughout the domain before disabling cal-

culation of the energy equation. If an unrealistic temperature value is used, the flow

properties dependent on temperature will also be unrealistic, and the flow field will be

adversely affected. Instructions for initializing the temperature field or patching a temper-

ature field onto an existing solution are provided in Initializing the Solution (p. ).

....Turning Reactions On and Off

To solve a species mixing problem prior to solving a reacting flow, you should set up the problem

including all of the reaction information, and save the complete case file. To turn off the reaction so

that only the species mixing problem can be solved, you can use the Species Model Dialog Box (p. )

to turn off the Volumetric option under Reactions.

Setup →

Models →

Once the species mixing problem has partially converged, you can return to the Species Model dialog

box and turn the Volumetric Reactions option on again. You can then resume the calculation starting

from the partially converged data.

For combustion problems you may want to patch a hot temperature in the vicinity of the anticipated

reactions before you restart the calculation. See Patching Values in Selected Cells (p. ) for information

about patching an initial value for a flow variable.

The default algebraic multigrid settings are appropriate for nearly all problems, but in rare cases you

may need to make minor adjustments. Setting Algebraic Multigrid Parameters (p. ) describes how

to analyze the multigrid solver’s performance to determine which parameters.

It is possible to make several changes to the multi-stage time-stepping scheme itself. See Changing

the Multi-Stage Scheme (p. ) for detailed information.

Poor quality meshes are meshes containing highly skewed cells, highly non-orthogonal cells, non-

convex cells, or cells with left-handed faces. Such mesh elements tend to decrease the numerical sta-

bility of traditional CFD discretization algorithms. These mesh elements require special treatment,

namely, a numerical correction of the transport equation discretization, which is intended to improve

the numerical properties of the solution algorithms at mesh cells of poor quality.

Note

If your mesh exhibits any type of poor quality except left-handed faces, you can maintain

second order accuracy by using the warped-face gradient correction and disabling poor

mesh numerics. To disable poor mesh numerics, set solve/set/poor-mesh-numer-

ics/enable? to no. For additional information on this method, see Warped-Face Gradient

Correction (p. ).

In order to facilitate solution convergence on meshes of poor quality, the ANSYS Fluent solver can

apply a local solution correction, limited spatially to distorted cells of the mesh. If you read in a poor

quality mesh containing cells and faces with corrupt metrics, you will see a warning in the TUI of the

form:

form:

Info: The mesh contains elements that are invalid or of poor quality.

A different numerical scheme will be applied to these elements,

which may affect the quality of the solution. It is recommended

that you consider removing the invalid and poor quality elements

For more information on the invalid and poor quality elements,

please use the following TUI commands:

/mesh/check

/mesh/repair-improve/report-poor-elements.

Additionally, in the Solution Methods task page, the Report Poor Quality Elements button will appear,

which can be used to report more statistics on the number and type of cells that ANSYS Fluent has

identified as having poor quality (see Figure . : Reporting Poor Quality Elements (p. )).

Figure . : Reporting Poor Quality Elements

apply a local solution correction, limited spatially to distorted cells of the mesh. The corrected solution

can be of 0th, 1st, or 2nd order:

The 0th order scheme applies an algorithm that computes the solution variable for the transport

equation in the bad cells by assembling the solution directly from the surrounding solution in the

better quality cells.

The 1st order scheme applies locally low order discretization methods and neglects some non-ortho-

gonal contributions to the gradients when computing the diffusive fluxes.

The 2nd order scheme only modifies the numerics in the bad cells by assembling the gradient vector

for the given solution variable from the gradients in the surrounding better quality cells.

In other words, the discretization error will be independent of the mesh size in this region if 0th order

is used. It will decrease linearly with subsequent grid refinement when 1st order is used, and quadrat-

ically when the 2nd order option is selected.

By default, Fluent will apply the 1st order correction scheme to any invalid cells. Using text commands,

you can further control the application of the poor mesh numerics by using one of the other schemes,

including highly skewed and highly non-orthogonal cells, and including cells from a user-defined register.

The text commands that are available are as follows:

/solve/set/poor-mesh-numerics/enable?

Choose whether or not to apply the poor mesh numerics corrections and specify which order scheme to

use.

In general, it is recommended that you use the 1st order solution correction, which provides a

reasonable compromise between accuracy and stability gain. For meshes of better (and yet still

low) quality it is advisable to try the 2nd order option, which will preserve the mesh convergence

behavior provided by the convection term discretization schemes. In case no convergence is ob-

tained with any of the aforementioned schemes, you should use the 0th order option, which will

provide the highest stability and at the same time the lowest accuracy. In regions with highly

nonlinear flow physics this scheme can yield highly nonphysical results.

The computational time (or cost or run time requirements) for all three schemes will increase linearly

as the number of cells identified as poor quality cells increases. Provided that there is reasonable

convergence behavior with all three schemes, the 1st order option will be the fastest; 0th and 2nd

order schemes will have similar run times to each other.

/solve/set/poor-mesh-numerics/cell-quality-based?

Choose whether or not the poor mesh numerics should also be applied to cells that are highly non-ortho-

gonal or highly skewed.

/solve/set/poor-mesh-numerics/set-quality-threshold

Set the threshold for including cells based on cell quality metrics when cell-quality-based? is

enabled.The value you enter is applied as a threshold for the cell orthogonality and the complement of

cell skewness below which the poor mesh numerics will be applied.The default value is .. Some

cases may require tuning this parameter to improve stability.

/solve/set/poor-mesh-numerics/user-defined-on-register

Answer yes at the prompt to Include cells from a register in the poor mesh numerics treatment.You will

be prompted for the name or ID of the register to include. Note that if you answer no at the prompt any

cells previously included from registers are removed from the list of cells for poor mesh numerics.

If you include a user-defined register in the poor mesh numerics, reporting of poor mesh element

statistics will also include the cells added by the user-defined-on-register command. For

example:

Poor Mesh Element Statistics:

Identified     faces with too small area.

Identified     faces adjacent to negative volume cells.

Identified     faces adjacent to bad quality cells.

Identified    cells from user-defined register.

Note

The statistics not only report the cells included in the register, but also their

Note

neighboring cells, resulting in an overall larger number of cells being identified.

Important

It is your responsibility to maintain the register-based cells. If you change the mesh,

(for example, using mesh manipulation or adaptation), then you must use the

user-defined-on-register command again. Enter yes to the command

prompt in order to update the cells based on a new cell register, otherwise, enter

no to remove all cells from the poor mesh numerics list. For more information

about cell registers, see Using Cell Registers (p. ).

/solve/set/poor-mesh-numerics/print-poor-elements-count

Print out a listing of the poor cells for each criterion (default, cell quality, and user-defined).

> /solve/set/poor-mesh-numerics/print-poor-elements-count

Number of marked cells based on default criteria       =

Number of marked cells based on cell quality criteria  =

Number of marked cells based on user-defined criteria  =

/solve/set/poor-mesh-numerics/reset-poor-elements?

Reset the poor cells included from user-defined registers and cell-quality metrics.The poor cells identified

from the internal mesh check will be retained.

The warped-face gradient correction (WFGC) is designed to improve gradient accuracy for all gradient

methods—cell based, node based and least squares based gradients. WFGC is recommended for 3D

simulations on polyhedral, hexahedral, and hybrid meshes (meshes containing a mix of hexahedral

and polyhedral cells), and it is enabled by default for any mesh that contains polyhedra. Note that

these types of mesh cells may not have perfectly planar faces, which can affect the overall accuracy

of the Green Gauss surface integral. WFGC is also recommended when you encounter numerical diffi-

culties in simulations that involve a mesh that has large differences in the volumes of neighboring

cells, such as hex cells with hanging node interfaces.

WFGC computations aim to resolve gradient accuracy degradation due to very high aspect ratio, cells

with non-flat faces in the boundary layer, and highly deformed cells where the formal cell centroid

lies outside of the control volume.

WFGC has two modes, fast mode and memory saving mode. Fast mode does not increase gradient

computation time for static meshes (except for cases that use the Green-Gauss Node Based gradient

method with a turbulence model), but it does require additional memory. There is roughly a % in-

crease in memory for a basic flow solution, but this additional overhead does not change as more

models (turbulence, species transport, radiation, and so on) are enabled. Memory saving mode does

not increase memory consumption, but it slows down iteration execution time for static and dynamic

meshes.

Important

Enabling Warped-Face Gradient Correction through the Solution Methods task page

enables fast mode. To switch to memory saving mode, you must use the TUI command

solve/set/warped-face-gradient-correction/enable? and enter no in re-

sponse to the use fast mode? prompt.

WFGC does not correct for cells with left-handed faces. If your mesh contains left-handed

faces, you must use poor mesh numerics to obtain a stable solution.

... Overview of Solution Steering

... Solution Steering Strategy

... Using Solution Steering

Solution steering in the density-based implicit solver provides you with an expert system that will help

navigate the flow solution from a starting initial guess to a converged solution with minimum user

interaction. When you apply solution steering, you will be required to select the type of flow that best

characterizes the solution domain and the maximum desired accuracy, and then allow the solver to

take the solution to convergence. As the solver proceeds with the solution iteration, certain solver

parameters will be adjusted behind the scenes to insure that a converged solution to steady-state is

possible.

Important

Solution steering is available only for steady-state flows in the density-based implicit solver.

The convergence to steady-state solution is achieved in two stages. The parameters that are used in

these stages are determined and set based on user input for the type of flow that can best characterize

the solution domain. The type of flows available for selection are classified based on flow compressib-

ility as well as the dominant flow Mach number in the solution domain.

The following flow types are available:

Incompressible (if the flow is incompressible, that is density is constant)

Subsonic (if the flow is compressible and M<.)

Transonic (if the flow is compressible and .<M<.)

Supersonic (if the flow is compressible and .< M<.)

Hypersonic (if the flow is compressible and .< M)

Important

There is no exact Mach number cut-off for these regions, therefore, the above Mach number

ranges are just a simple guideline to help you select a flow type.

Solution steering will typically perform full multigrid (FMG) initialization followed by two iterative

stages. The purpose of each stage is described below.

.... Initialization

Immediately before the start of the iteration, solution steering will perform full multigrid initialization

to obtain the best possible initial starting solution.

Stage :

The purpose of Stage  is to navigate the solution from the difficult initial phase of the solution toward

convergence by insuring maximum stability. During this stage, the solution is advanced gradually

from 1st-order accuracy to maximum accuracy (user specified and typically 2nd-order) at a constant

low CFL value.

Stage :

In this stage the solution is driven hard towards convergence by regular adjustments of the CFL value

to insure fast convergence as well as to prevent possible divergence.

In stage , the residual history is monitored and analyzed through regular intervals to determine if

an increase or decrease in CFL value is needed to obtain fast convergence or to prevent divergence.

Solution steering is disabled by default. However, when the following criteria are met, the solution

steering feature will become available for selection:

Setting

Feature

Density Based

Setting

Feature

Solver Type

Implicit

Solver Formulation

Steady

Time Formulation

Data is valid (either data file has been read or flow

has been initialized)

To turn on solution steering, enable the Solution Steering option as shown in Figure . : The Run

Calculation Task Page with Solution Steering Enabled (p. ).

Solution Steering

Figure . : The Run Calculation Task Page with Solution Steering Enabled

The Run Calculation task page will then expand to display the solution steering main controls (see

Figure . : The Run Calculation Task Page with Solution Steering Enabled (p. )). To obtain a flow

solution using solution steering, you will need to perform the following:

. Select the type of flow.

. Select the maximum accuracy desired (first- to second-order blending).

. Click Calculate.

You can also adjust the number of iterations, or customize the parameters of the solution steering if

the default setting is not sufficient for the type of flow problem being solved.

Before using solution steering, you will need to prepare and set up the case as usual as described in

the Fluent Getting Started Guide.

After Solution Steering is enabled, specify the following:

Flow Type

allows you to select the flow type that best describes the flow in the solution domain. Five choices are

available: incompressible, subsonic, transonic, supersonic, and hypersonic.

Use FMG Initialization

when enabled allows for full multigrid initialization before starting stages  and . FMG initialization is

First- to Higher-Order Blending

allows you to reduce the desired solution accuracy by selecting a blending factor less than %.The

default setting is %. See First- to Higher-Order Blending in the Theory Guide for more information.

The blending factor will be grayed out if Second Order Upwind discretization for the Flow equations is

not selected in the Solution Methods task page.The solution accuracy may be reduced (typical values

are % or %) if it is not possible to obtain a converged solution with the maximum second-order ac-

curacy (that is blending = %).

in the Run Calculation task page is a non-adjustable field displaying the current CFL number, which allows

you to view it during the calculation.

More Settings...

opens the Solution Steering dialog box, providing a host of settings that control the solution steering

strategy, as shown in Figure . :The Solution Steering Dialog Box (p. ).

Figure . : The Solution Steering Dialog Box

The Solution Steering dialog box, shown in Figure . : The Solution Steering Dialog Box (p. ),

contains two tabs. The Steering Settings tab sets the solution steering parameters and the FMG

Settings sets the full multigrid initialization parameters.

In the Steering Setting tab, you can modify the parameters used in Stages  and .

Stage

Duration is the number of iterations in stage .The CFL number used during these iterations is set in the

Initial field, in the Courant Number group box.

Stage

The Courant number update in stage  can start immediately after the end of stage , or after a certain

Stage

designated number of iterations. If the Courant number update is to start immediately after stage  then

Immediately should be selected (this is the default option). If the Courant number update is desired after

some lagged period of iterations, then After should be selected and the lag in the number of iterations

should be entered in the field below it.The frequency at which the Courant number is updated is defined

in Courant Number Update Interval field.

Initial is the starting Courant number and Maximum is the maximum allowed Courant number.The

solution steering algorithm will not allow the solver to exceed the maximum Courant number, but will

allow the solver to use a Courant number less than the initial Courant number if divergence in the solution

has occurred.

Explicit Under-Relaxation Factor

allows the solution to be under-relaxed to improve convergence.The under-relaxation value is determined

by the Flow Type that you selected in the Run Calculation task page, when Solution Steering was en-

abled. In general, you do not need to alter the default value set in this field. Refer to Under-Relaxation of

Variables in the Theory Guide for more information about explicit relaxation.

Default

is available in the Steering Settings tab to reset any changes made to the parameters to their original

In the FMG Settings tab (Figure . : The FMG Settings Tab in the Solution Steering Dialog Box (p. )),

the Number of multigrid levels and Number of Cycles in each Level, as well as the FMG Courant

Number used in the FMG initialization can be adjusted. The default values used in the multigrid settings

are determined from the type of flow that you selected, the size of the mesh, and the flow dimension-

ality. The Default button is used to reset any changes to the original default values. For more inform-

ation about FMG initialization, refer to Full Multigrid (FMG) Initialization (p. ).

Figure . : The FMG Settings Tab in the Solution Steering Dialog Box

Chapter : Adapting the Mesh

The solution-adaptive mesh refinement feature of ANSYS Fluent allows you to refine and/or coarsen

your mesh based on geometric and numerical solution data. In addition, ANSYS Fluent provides tools

for creating and viewing adaption fields customized to particular applications. For information about

the theory behind mesh adaption in ANSYS Fluent, see Adapting the Mesh in the Theory Guide. Inform-

ation about using the adaption process in ANSYS Fluent is described in detail in the following sections.

.. Using Adaption

.. Refining and Coarsening

.. Adaption Examples

.. Anisotropic Adaption

.. Geometry-Based Adaption

Two significant advantages of the unstructured mesh capability in ANSYS Fluent are:

reduced setup time compared to structured meshes

the ability to incorporate solution-adaptive refinement of the mesh

By using solution-adaptive refinement, you can add cells where they are needed in the mesh, thus en-

abling the features of the flow field to be better resolved. When adaption is used properly, the resulting

mesh is optimal for the flow solution because the solution is used to determine where more cells need

to be added. Thus, computational resources are not wasted by the inclusion of unnecessary cells, as

occurs in the structured mesh approach. Also, the effect of mesh refinement on the solution can be

studied without completely regenerating the mesh.

Note

When you are running in parallel, Fluent performs load balancing, which redistributes cells

across compute nodes. Refer to Partitioning the Mesh Automatically (p. ) and Load Balan-

cing (p. ) for additional information on load balancing. After the mesh is adapted, Fluent

automatically performs a load balancing step, by default.

For more information about the adaption process, see Adaption Process in the Theory Guide.

See the following sections for information on performing mesh adaption:

... Adaption Example

... Adaption Guidelines

An example of the effective use of adaption is in the solution of the compressible, turbulent flow

through a 2D turbine cascade. The initial mesh around the blade is fine, as shown in Figure . : Turbine

Cascade Mesh Before Adaption (p. ). The surface node distribution thus provides adequate definition

of the blade geometry, and enables the turbulent boundary layer to be properly resolved without

further adaption. On the other hand, the mesh on the inlet, outlet, and periodic boundaries is compar-

atively coarse. To ensure that the flow in the blade passage is appropriately resolved, solution-adaptive

refinement was used to create the mesh shown in Figure . : Turbine Cascade Mesh after Adap-

tion (p. ).

tion (p. ).

Figure . : Turbine Cascade Mesh Before Adaption

Figure . : Turbine Cascade Mesh after Adaption

While the procedure for solution adaption will vary according to the flow being solved, it is instructive

to examine the adaption process used for the turbine cascade shown in the previous figure. Though

this example involves compressible flow, the general procedure is applicable for incompressible flows

as well.

Adapting the Mesh

. Display contours of pressure to determine a suitable refinement threshold.

. Mark the cells within the refinement threshold, creating a refinement register (see Field Variable (p. )).

. Repeat the process described in steps  and , using gradients of Mach number as a refinement criterion.

. To refine in the wake region, use isovalues of total pressure as a criterion (see Field Variable (p. )).This

causes cells within the boundary layer and the wake to be marked, since these are both regions of high

total-pressure loss.

. Refine the cells contained in the register (see Refining and Coarsening (p. )).

The effect of refining on gradients is evident in the finer mesh ahead of the leading edge of the blade

and within the blade passage (Figure . : Turbine Cascade Mesh after Adaption (p. )). The finer

mesh in the wake region is due to the adaption using isovalues of total pressure.

The advantages of solution-adaptive refinement, when used properly (as in the turbine cascade example

in Adaption Example (p. )), are significant. However, this capability must be used carefully to avoid

certain pitfalls. Some guidelines for proper usage of solution-adaptive refinement are as follows:

The surface mesh must be fine enough to adequately represent the important features of the geometry.

For example, it would be bad practice to place too few nodes on the surface of a highly-curved

airfoil, and then use solution refinement to add nodes on the surface. The surface will always contain

the facets contained in the initial mesh, regardless of the additional nodes introduced by refinement.

The initial mesh should contain sufficient cells to capture the essential features of the flow field.

Consider the following example, in which you want to predict the shock forming around a bluff

body in supersonic flow. To obtain a reasonable first solution, the initial mesh should contain enough

cells and also have sufficient resolution to represent the shape of the body. Subsequent gradient

adaption can be used to sharpen the shock and to establish a mesh-independent solution.

Polyhedral cells are only eligible for adaption with the polyhedral unstructured mesh adaption

(PUMA) method.

For the default hanging node adaption method, the presence of polyhedral cells in a mesh may or

may not limit the eligibility of other cells for adaption, depending on the manner in which the

polyhedral cells were created:

– If the domain was converted to polyhedra (see Converting the Domain to a Polyhedra (p. )), then no

part of the mesh can be adapted (even if hexahedral cells are present in the mesh after conversion).

– If the polyhedra are a result of converting skewed tetrahedral cells (see Converting Skewed Cells to

Polyhedra (p. )) or converting the transitional cells of a hexcore mesh, then the non-polyhedral cells

may be adapted.The polyhedral cells, however, will be automatically unmarked from the register when

adaption is initiated and will remain unchanged.

Obtain a reasonably well-converged solution before performing an adaption. If you adapt to an incorrect

solution, cells will be added in the wrong region of the flow.

Use careful judgment in deciding how well to converge the solution before adapting, because there

is a trade-off between adapting too early to an unconverged solution and wasting time by continuing

Using Adaption

to iterate when the solution is not changing significantly. This does not directly apply to dynamic

adaption, because here the solution is adapted either at every iteration or at every time step, de-

pending on which solver is being used.

Write a case and data file before starting the adaption process. If you generate an undesirable mesh, you

can restart the process with the saved files.This does not directly apply to dynamic adaption, because here

the solution is adapted either at every iteration or at every time step, depending on which solver is being

used.

Select suitable variables when performing gradient adaption. For some flows, the choice is clear. For instance,

adapting on gradients of pressure is a good criterion for refining in the region of shock waves. In most in-

compressible flows, however, it makes little sense to refine on pressure gradients. A more suitable parameter

in an incompressible flow might be mean velocity gradients. If the flow feature of interest is a turbulent

shear flow, it will be important to resolve the gradients of turbulent kinetic energy and turbulent energy

dissipation, so these might be appropriate refinement variables. In reacting flows, temperature or concen-

tration (or mole or mass fraction) of reacting species might be appropriate.

Do not over-refine a particular region of the solution domain. It causes very large gradients in cell volume.

Such poor adaption practice can adversely affect the accuracy of the solution.

You can refine or coarsen your mesh based on cell registers (Using Cell Registers (p. )) using the

Adaption Controls dialog box.

To setup mesh adaption:

. Create cell registers for the types of cells that you want to adapt (Using Cell Registers (p. )).

Solution → Cell Registers

New

. Open the Adaption Controls dialog box.

Domain → Adapt → Refine / Coarsen

Figure . : The Adaption Controls Dialog Box

. Specify the Refinement Criterion you want Fluent to use to determine when the mesh should be refined.

You can specify either a cell register or provide an expression.

. Specify the Coarsening Criterion you want Fluent to use to determine when the mesh should be coarsened.

. Specify the Maximum Refinement Level, which controls the number of levels of refinement used to split

cells during the adaption. The default of  is a good start for most problems.This field essentially keeps Fluent

from infinitely refining the mesh. Specifying too large of a value can quickly lead to a very large cell count.

. Set the Minimum Cell Volume.This field restricts the size of cell that Fluent considers for refinement. Even

if the cell is marked for refinement, it will not be refined if its cell volume is less than this threshold value.

. (Optional) Enable Dynamic Adaption to have Fluent automatically adapt the mesh while the calculation

is proceeding.

a.

Specify how frequently Fluent can adapt the mesh by setting the Frequency to the number of iterations

or time steps that must pass between two consecutive automatic mesh adaptions.

. (Optional) Enable Advanced Controls to specify the number of Additional Refinement Layers that can

be adapted. Figure . : Additional Refinement Layers: , ,  (p. ) shows how this functionality in action.

. (Optional) Click List Criteria to print the number of cells that Fluent has identified for being refined,

coarsened, or both, to the console.

. (Optional) Click Display to review the cells that are marked for adaption.

. Click OK to save the adaption control settings or click Adapt to adapt the mesh.

Refining and Coarsening

Additional Refinement Layers (Transient Cases Only)

You have the option to add more refinement layers during adaption, as shown in Figure . : Additional

Refinement Layers: , ,  (p. ).

Figure . : Additional Refinement Layers: , ,

The following are examples of adapting the mesh based on different types of cell registers and one

using just expressions.

... Boundary Cell Register

... Region Cell Register

... Field Variable Cell Registers (gradients, scaling, and so on)

... Expression Adaption Refinement

If more cells are required on a boundary, they can be added using boundary adaption, which allows

you to mark or refine cells in the proximity of the selected boundary zones. The ability to refine the

mesh near one or more boundary zones is provided because important fluid interactions often occur

in these regions (for example, the development of strong velocity gradients in the boundary layer near

a wall).

An example of a mesh that can be improved with boundary adaption is shown in Figure . : Mesh

Before Adaption (p. ). This mesh has only four cells on the vertical face of a step.

To mark cells for refinement, you can create a boundary cell register (Boundary (p. )), as shown in

Figure . : Marking Boundary Cells (p. ).

Figure . : Marking Boundary Cells

Boundary adaption on the zone corresponding to the face of the step can be used to increase the

number of cells, as shown in Figure . : Mesh after Boundary Adaption (p. ). This procedure cannot

increase the resolution of a curved surface. Therefore, if more cells are required on a curved surface

where the shape of the surface is important, create the mesh with sufficient surface nodes before

reading it into the solver.

Adaption Examples

Figure . : Mesh Before Adaption

Figure . : Mesh after Boundary Adaption

Figure . : Wing Mesh Before Adaption (p. ) shows a mesh that was created for solving the flow

around an airfoil wing. The mesh is fine near the surface of the wing. To capture the flow separation

that occurs on the surface of the wing lip, the mesh is refined after marking cells within a circular region

(selected by mouse probe) surrounding the lip of the wing. Figure . : Marking Cells Based on Re-

gion (p. ) shows the settings that are used to mark the cells in the wake region.

Figure . : Wing Mesh Before Adaption

Figure . : Marking Cells Based on Region

The resulting adapted mesh is shown in Figure . : Wing Mesh After Region Cell Register-Based

Adaption (p. ).

Figure . : Wing Mesh After Region Cell Register-Based Adaption

Direct error estimation for point-insertion adaption schemes is difficult because of the complexity of

accurately estimating and modeling the error in the adapted meshes. A comprehensive mathematically

rigorous theory for error estimation and convergence is not yet available for CFD simulations. Assuming

that maximum error occurs in high-gradient regions, the readily available physical features of the

evolving flow field may be used to drive the mesh adaption process.

When using the Scaling Option, suitable first-cut values for the Cells More Than and the Cells Less Than

are . to ., and . to ., respectively. Smaller values will result in larger adapted regions.

Scale by Global Maximum, scales the values of

,

, or

by their maximum value in the domain,

therefore always returning a problem-independent range of [, ] for any variable used for adaption, that

is:

(.)

When using the Scale by Global Maximum option, suitable first-cut values for the Coarsening

threshold and the refinement threshold are . to ., and . to ., respectively. Smaller values

will result in larger adapted regions.

When you are using the derivative and scaling options, you can create a refinement register, like the

one shown in Figure . : Field Variable Refinement Register (p. ).

Figure . : Field Variable Refinement Register

Then, using the Cells Less Than type of field variable register, you can create a coarsening cell register,

as shown in Figure . : Field Variable Coarsening Register (p. ).

Figure . : Field Variable Coarsening Register

These cell registers can then be combined in the Adaption Controls dialog box to define parameters

for adaption, as shown in Figure . : Controls for Refining and Coarsening the Mesh (p. ).

Figure . : Controls for Refining and Coarsening the Mesh

There are several ways to use expressions to perform adaption. Expressions can be used with or without

cell registers to define refinement and coarsening criteria, as shown in Figure . : Simple Expression

Refinement Setting (p. ) and Figure . : Advanced Expression Refinement Setting (p. ).

Figure . : Simple Expression Refinement Setting

Figure . : Cells Marked for Simple Expression Refinement

Figure . : Advanced Expression Refinement Setting

Figure . : Cells Marked for Advanced Expression Refinement

Combined Boolean Operation and Variables

You can combine booleans with various postprocessing variables. For example, AND(OR(Static-

Pressure<. [Pa], CellRefineLevel<), CellVolume>1e-[m^])

Combined Boolean Operation and Cell Register

If you want to refine cells near an outlet where the pressure is less than p0, you can use an expression:

AND(Pressure<p0 [Pa], near_outlet_cells). Here, p0 is a constant real value and

near_outlet_cells is a boundary cell register with specified values (refer to Boundary (p. ) for

additional information on boundary cell registers).

This section describes how to perform anisotropic adaption. For more information, see Anisotropic Ad-

aption in the Theory Guide.

... Limitations of Anisotropic Adaption

... Performing Anisotropic Adaption

Anisotropic Adaption

... Boundary Layer Redistribution

Since anisotropic adaption is available only for specific cell types, the following limitations exist:

It is only available in 3D.

It only works for hexahedral cells or prism cells.

Each cell can only be split into two, with a given splitting ratio in the normal direction of the boundary

face. Multiple layers can be achieved by multiple refinement.

Each cell to be split can only be reached once from any of the boundary faces; otherwise, the refinement

will not be processed.

Unlike other adaption functionalities, the subdivided cells cannot be coarsened again, because all the cells

that are adjacent to the refined cells are converted into polyhedral cells.

You will perform anisotropic adaption in the Anisotropic Adaption Dialog Box (p. ) (Figure . : The

Anisotropic Adaption Dialog Box (p. )).

Setting Up Domain → Adapt → More → Anisotropic Refinement...

Figure . : The Anisotropic Adaption Dialog Box

The procedure for performing anisotropic adaption is as follows:

. In the Anisotropic Adaption Dialog Box (p. ), select Cell Distance or Register from the Cell Options

group box.This allows you to control the marking of boundary layer cells. Select Cell Distance and enter

the Number of Cells to be adapted and marked using the distance from the boundary zone. Select Register

to adapt and mark cells using an existing Register.

. The Splitting Options control how the splitting ratio is computed. It is defined as follows:

By default, Automatic is selected, resulting in the ratio being computed automatically from the

mesh. If you selected Manual, enter the desired Split Ratio. If you choose to compute the split

ratio automatically, the split ratio of the first layer is computed, and it may be . if the original

cells are uniformly distributed, resulting in the height of the first layer being the same as the height

of the second layer.

Important

Note that the Split Ratio that you enter is only applicable to the first layer, and all the

other layers are split with a ratio of ..

. For the Cell Distance option, one or more boundary face zones must be selected before marking the cells

for refinement.

. For the Register option, select a register in the list. Note that one or more boundary face zones must be

selected before doing the refinement.

. Click Refine to refine the marked cells.

After performing anisotropic adaption the boundary layer zone will generally not satisfy the original

growth rate. To restore the desired growth rate you can use the mesh/redistribute-boundary-

layer TUI command. You will be prompted to enter a face zone and the desired growth rate. The

face zone you specify must be adjacent to the boundary layer zone that you want to redistribute.

>  mesh redistribute-boundary-layer

face zone id/name [] wall-fluid

growth rate [.] .

Fluent will redistribute the nodes in a boundary region that extends into the mesh from the face zone

you specify until one of the following criteria is encountered:

the edge of the domain

a change in zone

a change in element type

As with anisotropic adaption itself, boundary layer redistribution is only available in 3D problems.

This section describes how to perform geometry-based adaption. For more information, see Geometry-

Based Adaption in the Theory Guide.

... Performing Geometry-Based Adaption

Geometry-Based Adaption

The Geometry Based Adaption Dialog Box (p. ) (Figure . : The Geometry Based Adaption Dialog

Box (p. )) allows you to reconstruct the geometry while performing boundary adaption.

Setting Up Domain → Adapt → More → Geometry...

Figure . : The Geometry Based Adaption Dialog Box

The procedure for performing geometry-based adaption is as follows:

. Under Wall Zones, select the zone you want to adapt and click Set....The Geometry Based Adaption

Controls Dialog Box (p. ) will open.

Figure . : The Geometry Based Adaption Controls Dialog Box

In the Geometry Based Adaption Controls Dialog Box (p. ), set the following parameters:

Specify Levels of Projection Propagation to indicate the number of layers of the nodes you want to

project.

Enable Direction of Projection and specify the directions in which you want to project the nodes.

This will make the X , Y , and Z fields available. If you want node projection in the X direction, enter

for X . If you do not enable this option, the node projection will take place at the nearest point.

(optional) If you have a fine surface mesh for the geometry, you can use the Background Mesh option

to load the surface mesh as a background mesh.This will project the nodes based on the background

mesh and reconstruct the geometry more accurately.

To disable the geometry reconstruction for any zone in the domain, enable the Disable Geometry

Based Adaption for this Zone option.

. To disable geometry-based adaption for the whole domain, disable Reconstruct Geometry.

After setting the parameters for geometry-based adaption, proceed to perform mesh adaption.

Chapter : Creating Surfaces and Cell Registers for Displaying and

Reporting Data

ANSYS Fluent enables you to select portions of the domain to be used for visualizing the flow field. The

domain portions are called surfaces, and there are many ways to create them. Surfaces are required for

graphical analysis of 3D problems because you cannot display vectors, contours, and so on, or create

an XY plot for the entire domain at once. In 2D you can usually visualize the flow field on the entire

domain, but to create an XY plot of a variable in a portion of the interior of the domain, you must

generate a surface. In addition, in both 2D and 3D, you will need one or more surfaces if you want to

generate a surface-integral report. Note that ANSYS Fluent will automatically create a surface for each

boundary zone in the domain. Surface information is stored in the case file.

While you can create surfaces to visualize portions of the domain, you can create cell registers to visu-

alize and perform operations on cell groupings. You can group cells by:

Region

Boundary

Variable Limiter

Field Variable

Residuals

Volume

Yplus/Ystar

Cell registers are saved with the case file and can be used to display marked cells, adapt the mesh, apply

poor mesh numerics, and report on the cells.

The following sections explain creating surfaces and cell registers:

.. Using Surfaces

.. Using Cell Registers

In order to visualize the internal flow of a 3D problem or create XY plots of solution variables for 3D

results, you must select portions of the domain (surfaces) on which the data is to be displayed. Surfaces

can also be used for visualizing or plotting data for 2D problems, and for generating surface-integral

reports.

ANSYS Fluent allows you to create several kinds of surfaces, and stores all surfaces in the case file. You

can create the surfaces through the ribbon and the outline view and you can review and modify the

existing surfaces in the outline view under the Results branch. These surfaces and their uses are described

briefly below:

Zone Surfaces:

If you want to create a surface that will contain the same cells/faces as an existing cell/face zone, you can

generate a zone surface.This kind of surface is useful for displaying results on boundaries.

Partition Surfaces:

When you are using the parallel version of ANSYS Fluent, you may find it useful to create surfaces that are

defined by the boundaries between mesh partitions.You can then display data on each side of a partition

boundary.

See Parallel Processing (p. ) for more information about running the parallel solver.

Point Surfaces:

To monitor the value of some variable or function at a particular location in the domain, you can create a

surface consisting of a single point.

Structural Point Surfaces:

To monitor the value of some variable or function at a point in a particular cell of a solid zone in a

simulation that uses the structural model, you can create a surface consisting of a single point. For

example, you could monitor the displacement of a solid cell as it moves / deforms as part of a two-

way intrinsic fluid-structure interaction (FSI) simulation.

Line and Rake Surfaces:

To generate and display pathlines, you must specify a surface from which the particles are released. Line

and rake surfaces are well-suited for this purpose and for obtaining data for comparison with wind tunnel

data. A rake surface consists of a specified number of points equally spaced between two specified end-

points. A line surface is simply a line that includes the specified endpoints and extends through the domain;

data points will be at the centers of the cells through which the line passes, and consequently will not be

equally spaced.

Plane Surfaces:

If you want to display flow-field data on a specific plane in the domain, you can create a plane surface. A

plane surface is simply a plane that passes through three specified points.

Quadric Surfaces:

To display data on a line (2D), plane (3D), circle (2D), sphere (3D), or quadric surface you can specify the

surface by entering the coefficients of the quadric function that defines it.This feature provides you with

an explicit method for defining surfaces.

Isosurfaces:

You can use an isosurface to display results on cells that have a constant value for a specified variable.

Generating an isosurface based on ,

, or  coordinate, for example, will give you an ,

, or  cross-

section of your domain. Generating an isosurface based on pressure will enable you to display data for

another variable on a surface of constant pressure.

Note

In some instances, newly created surfaces (except zone/line/point/rake) may contain erroneous

lines. This can happen for surfaces created in any type of cell zone, but it is more likely in

zones containing polyhedral mesh elements. Displaying a contour plot on these surfaces or

displaying the surfaces directly may show these line edges. To reduce their appearance you

can change the lighting method to Flat.

Creating Surfaces and Cell Registers for Displaying and Reporting Data

... Zone Surfaces

Zone surfaces are useful for displaying results on boundaries. For example, you may want to plot

contours of velocity magnitude at the inlet and outlet of the problem domain, or temperature contours

on the domain’s walls. To do so, you need to have a surface that contains the same faces (or cells) as

an existing face (or cell) zone. Zone surfaces are created automatically for all boundary face zones in

the domain, so you will generally not need to create any zone surfaces unless you accidentally delete

one.

Use the text command: surface/reset-zone-surfaces to recreate any missing surface zones

by resetting the case surface list.

To create a zone surface, you will use the Zone Surface Dialog Box (p. ) (Figure . : The Zone Surface

Domain → Surface → Create → Zone...

Figure . : The Zone Surface Dialog Box

The steps for creating the zone surface are as follows:

.

Select the zone(s) in the Zone list.

.

Enter a name in New Surface Name if you do not want ANSYS Fluent to assign a default name to the

newly created surface. By default, Fluent assigns each surface the same name as the zone that it corres-

ponds to. If a surface already exists with that name, Fluent assigns the surface a unique name using the

zone-surface prefix (for example, zone-surface-).

Using Surfaces

If you do not want to use the default name, enter a new name in New Surface Name. If the New

Surface Name that you enter is the same as a surface that already exists, Fluent assigns the new

surface a unique name using the zone-surface prefix (for example, zone-surface-).

Important

The surface name that you enter must begin with an alphabetical letter. If your surface

Important

name begins with any other character or number, Fluent  rejects the entry.

If you are selecting multiple zones, you do not have the option to choose the surface names.

ANSYS Fluent automatically give the surfaces the same names as their corresponding zone.

.

Click Create.The new surface name is added to the Surfaces list in the dialog box.

If you want to delete or otherwise manipulate any surfaces, click Manage... to open the Surfaces Dialog

Box (p. ). For details, see Grouping, Editing, Renaming, and Deleting Surfaces (p. ).

... Partition Surfaces

If you are using the parallel version of ANSYS Fluent (see Parallel Processing (p. )), you may find it

useful to create data surfaces defined by the boundaries of mesh partitions. As described in Mesh

Partitioning and Load Balancing (p. ), partitioning the mesh divides it into groups of cells that can

be solved on separate processors when you use a parallel solver. A partition surface will contain faces

or cells on the boundary of two mesh partitions. For example, you can plot solution values on the

partition surface to determine how the solution is changing across a partition interface, as shown in

the following figure:

Figure . : Contours of Cell Partitions on Partition Surface Overlaid on Mesh

To create a partition surface, you will use the Partition Surface Dialog Box (p. ) (Figure . : The

Partition Surface Dialog Box (p. )).

Domain → Surface → Create → Partition...

Figure . : The Partition Surface Dialog Box

The procedure for creating the partition surface are as follows:

.

Specify the partition boundary in which you are interested by indicating the two bordering partitions

under the Partitions heading.The boundary that defines the partition surface is the boundary between

the "interior partition" and the "exterior partition". Int Part indicates the ID number of the interior partition

(that is, the partition under consideration), and Ext Part indicates the ID number of the bordering (exter-

ior) partition.The Min and Max fields will indicate the minimum and maximum ID numbers of the mesh

partitions.The minimum is always zero, and the maximum is one less than the number of processors. If

there are more than two mesh partitions, each interior partition will share boundaries with several exter-

ior partitions. By setting the appropriate values for Int Part and Ext Part, you can create surfaces for any

of these boundaries.

.

Choose interior or exterior faces or cells to be contained in the partition surface by selecting or clearing

Cells and Interior under Options.To obtain a surface consisting of cells that are on the "interior" side

of the partition boundary, select both Cells and Interior.To create one consisting of cells that are on

the "exterior" side, select Cells and clear Interior. If you want the surface to contain the faces on the

boundary instead of the cells, clear the Cells option.To have the faces reflect data values for the interior

cells, select the Interior check box, and to have them reflect values for the exterior cells, clear it.

.

.

If you do not want to use the default name assigned to the surface, enter a new name under New Surface

Name.The default name is the concatenation of the surface type and an integer that is the new surface

ID (for example, partition-surface-). (If the New Surface Name you enter is the same as the

name of a surface that already exists, ANSYS Fluent will automatically assign the default name to the

new surface when it is created.)

Important

The surface name that you enter must begin with an alphabetical letter. If the name

of the surface begins with any other character or number, ANSYS Fluent rejects the

entry.

.

... Imprint Surfaces

If you want to display results on surfaces that are more complicated than a simple point or plane, then

you can import a custom surface representing the region of interest (.stl or .msh format) and “im-

print” this surface into the current mesh. For example, you may want to visualize only a smaller custom

portion of a much larger (complex) geometry.

To create an imprinted surface, use the Imprint Surface Dialog Box (p. ) (Figure . : The Imprint

Surface Dialog Box (p. )).

Domain → Surface → Create → Imprint...

Figure . : The Imprint Surface Dialog Box

Create an imprinted surface as follows:

.

.

Click Read and select your geometry file (.stl or .msh format) using the Select File dialog box.

.

Click OK to upload your file.

The name of your geometry file appears in the Imported Surface dialog box.

.

Select the zone where your geometry is located in the From Zones group box.

Note

If you do not specify a zone, Fluent uses the entire domain for imprinting. For a large

mesh this could be time consuming.

.

Enter a name for your new surface in the New Surface Name dialog box.

The default name is <orig-name>(imprint)<id>.

.

Click Create to create the new surface.

When an imported surface is imprinted, a postprocessing surface that coincides with the imported

surface is created. The imprinted surface will not have facets for the portions of the original surface

that lie outside the domain. Different postprocessing operations such as contour and vector plots, and

surface integrals can be performed on this surface. However, the edges of the imprinted surface may

not coincide with those of the original surface, if the edges of the original surface do not coincide

with mesh edges. An example is shown in the following picture.

Figure . : Imprinted Surface (pink) Superimposed Over Imported Surface (white)

As you can see in Figure . : Imprinted Surface (pink) Superimposed Over Imported Surface

(white) (p. ), there are deformities around the edges of the imprinted surface.

Important

If you want to create an imprint surface from multiple disconnected source surfaces, it is

Important

better to create multiple imprint surfaces (one per source surface) and, if required, group

them together after they are created. For information on grouping surfaces, see Grouping,

Editing, Renaming, and Deleting Surfaces (p. ).

... Point Surfaces

You may often be interested in displaying results at a single point in the domain. For example, you

may want to monitor the value of some variable or function at a particular location. To do this, you

must first create a "point" surface, which consists of a single point. When you display node-value data

on a point surface, the value displayed is a linear average of the neighboring node values. If you display

cell-value data, the value at the cell in which the point lies is displayed.

To create a point surface, use the Point Surface Dialog Box (p. ) (Figure . : The Point Surface Dialog

Box (p. )).

Domain → Surface → Create → Point...

Figure . : The Point Surface Dialog Box

Create a point surface as follows:

.

Specify the location of the point.There are three different ways to do this:

Enter the coordinates (x0, y0, z0) under Coordinates.

Click Select Point With Mouse and then select the point by clicking on a location in the active

graphics window with the mouse-probe button. (See Controlling the Mouse Button Functions (p. )

for information about setting mouse button functions.)

Use the Point Tool option to interactively position a point in the graphics window.You can set the

initial location of this point using one of the two methods described above for specifying the point’s

position (or you can start from the position defined by the default Coordinates). See Using the Point

Tool (p. ) for information about using the point tool.

.

ID (for example, point-). (If the New Surface Name you enter is the same as the name of a surface

that already exists, ANSYS Fluent will automatically assign the default name to the new surface when it

is created.)

Important

entry.

.

If you want to check that your new surface has been added to the list of all defined surfaces, or you

want to delete or otherwise manipulate any surfaces, click Manage... to open the Surfaces Dialog

Box (p. ). For details, see Grouping, Editing, Renaming, and Deleting Surfaces (p. ) for details.

.... Using the Point Tool

The point tool enables you to interactively fine-tune the definition of a point using graphics. Starting

from an initial point, you can translate the point until its position is as desired. For example, if you

need to position a point surface at the center of a duct, just past the inlet, you can start with the

point tool near the desired location (such as on the inlet), and translate it until it is in the proper

place. (You may find it helpful to display mesh faces to ensure that the point tool is correctly positioned

inside the domain.)

..... Initializing the Point Tool

Before enabling the Point Tool option, set the Coordinates to suitable starting values. You can

enter values manually, or use the Select Point With Mouse button. Often it is convenient to display

the mesh for an inlet or isosurface on or near where the point is to be located, and then select a

point on that mesh to specify the initial position of the point tool. Once you have specified the ap-

propriate Coordinates, turn on the tool by enabling the Point Tool option. The point tool, an eight-

sided polygon, will appear in the graphics window, as shown in Figure . : The Point Tool (p. ).

Figure . : The Point Tool

You can then translate the point tool as described below. The point surface you create will be located

at the center of the point tool.

.....Translating the Point Tool

To translate the point tool in the direction along the red axis, click the mouse-probe button (the

right button by default) anywhere on the gray part of the point tool and drag the mouse until the

tool reaches the desired location. Green arrows will show the direction of motion. For information

about changing the mouse functions, see Controlling the Mouse Button Functions (p. ).

To translate the tool in the transverse directions (that is, along either of the other axes), press Shift,

click the mouse-probe button anywhere on the gray part of the point tool, and drag the mouse

until the tool reaches the desired location. Two sets of green arrows will show the possible directions

of motion. In 2D, there will be only one set of green arrows because there is only one other direction

for translation. If you find the perspective distracting when performing this type of translation, you

can turn it off in the Camera Parameters Dialog Box (p. ) (opened from the Views Dialog Box (p. )),

as described in Controlling Perspective and Camera Parameters (p. ).

..... Resetting the Point Tool

If you "lose" the point tool, or want to reset it for any other reason, you can either click Reset to

return the point tool to the default position and start from there, or turn the tool off and re-initialize

it as described above. In the default position, the point tool will lie at the center of the domain.

... Structural Point Surfaces

You may be interested in reporting data at a point in a particular cell of a solid zone in a simulation

that uses the structural model. For example, you may want to monitor the displacement of a solid cell

as it moves / deforms as part of a two-way intrinsic fluid-structure interaction (FSI) simulation. To do

this, you must first create a structural "point" surface, which consists of a single point. When you display

node-value data on a structural point surface, the value displayed is a linear average of the neighboring

node values. If you display cell-value data, the value at the cell in which the point lies is displayed.

To create a structural point surface, use the Point Surface Dialog Box (p. ) (Figure . : The Structural

Point Surface Dialog Box (p. )).

Domain → Surface → Create → Structural Point...

Figure . : The Structural Point Surface Dialog Box

Create a structural point surface as follows:

.

Note

The point must be in a solid cell zone. The structural model must also be enabled for

the Structural Point Surface dialog box to be available (refer to Modeling Fluid-

Structure Interaction (FSI) Within Fluent (p. ) for additional information).

.

ID (for example, structural-point-). (If the New Surface Name you enter is the same as the name

of a surface that already exists, ANSYS Fluent will automatically assign the default name to the new surface

when it is created.)

Important

Important

entry.

.

... Line and Rake Surfaces

You can create lines and rakes in the domain for releasing particles, obtaining data for comparison

with tunnel data, and so on. A rake consists of a specified number of points equally spaced between

two specified endpoints. A line is simply a line that extends up to and includes the specified endpoints;

data points will be located where the line intersects the faces of the cell, and consequently may not

be equally spaced.

To create a line or rake surface, you will use the Line/Rake Surface Dialog Box (p. ) (Figure . : The

Line/Rake Surface Dialog Box (p. )).

Domain → Surface → Create → Line/Rake...

Figure . : The Line/Rake Surface Dialog Box

The steps for creating the line or rake surface are as follows:

.

Indicate whether you are creating a Line surface or a Rake surface by selecting the appropriate item in

the Type drop-down list.

.

If you are creating a rake surface, specify the Number of Points to be equally spaced between the two

endpoints.

.

.

.

Specify the location of the line or rake surface.There are three different ways to define the location:

Enter the coordinates of the first point (x0, y0, z0) and the last point (x1, y1, z1) under End Points.

Click Select Points With Mouse and then select the endpoints by clicking on locations in the active

Use the Line Tool option to interactively position a line in the graphics window.You can set the initial

location of this line using one of the two methods described above for specifying endpoints (or you

can start from the position defined by the default End Points). See Using the Line Tool (p. ) for in-

formation about using the line tool.

Note that when you use the second or third method described above, the coordinates of the End

Points are updated automatically.

.

ID (for example, line- or rake-). If the New Surface Name you enter is the same as the name of

a surface that already exists, ANSYS Fluent will automatically assign the default name to the new surface

when it is created.

Important

entry.

.

entry.

.

If you want to check that the new surface has been added to the list of all defined surfaces, or you

Box (p. ). See Grouping, Editing, Renaming, and Deleting Surfaces (p. ) for details.

.... Using the Line Tool

The line tool enables you to interactively fine-tune the definition of a line or rake using graphics.

Starting from an initial line, you can translate, rotate, and resize the line until its position, orientation,

and length are as desired. For example, if you need to position a rake surface just inside the inlet to

a duct, you can start with the line tool near the desired location (such as on the inlet), and translate,

rotate, and resize it until you are satisfied. You may find it helpful to display mesh faces to ensure

that the line tool is correctly positioned inside the domain.

..... Initializing the Line Tool

Before enabling the Line Tool option, set the End Points to suitable starting values. You can enter

values manually, or use the Select Points With Mouse button. Often it is convenient to display the

mesh for an inlet or isosurface on or near where you want to place the line or rake surface and then

select two points on that mesh to specify the initial position of the line tool. Once you have specified

the appropriate End Points, enable the Line Tool option. The line tool appears in the graphics

window, as shown in Figure . : The Line Tool (p. ).

Figure . : The Line Tool

You can then translate, rotate, and/or resize the line tool as described in the following sections.

.....Translating the Line Tool

To translate the line tool in the direction along the red axis, click the mouse-probe button (the right

button by default) anywhere on the “line” part of the tool and drag the mouse until the tool reaches

the desired location. Green arrows will show the direction of motion For information about changing

the mouse functions see Controlling the Mouse Button Functions (p. ).

Important

Do not click the axes of the line tool that have arrows on the ends. These axes control

rotation of the tool. Click only on the portion of the tool that represents the prospective

line surface. This portion is designated by the rectangles attached to each end.

To translate the tool in the transverse directions (that is, along either of the axes within the plane

perpendicular to the red axis), press Shift, click the mouse-probe button anywhere on the "line" part

of the tool, and drag the mouse until the tool reaches the desired location. Two sets of green arrows

will show the possible directions of motion. In 2D, there will be only one set of green arrows because

there is only one other direction for translation. If you find the perspective distracting when perform-

ing this type of translation, you can disable it in the Camera Parameters Dialog Box (p. ) (opened

from the Views Dialog Box (p. )), as described in Controlling Perspective and Camera Paramet-

ers (p. ).

..... Rotating the Line Tool

To rotate the line tool, you click the mouse-probe button on one of the white axes with arrows.

ers (p. ).

When you click one of these axes, a green ribbon will encircle the other arrowed axis, designating

it as the axis of rotation. As you drag the mouse along the circle to rotate the tool, the green circle

will become yellow.

Important

Do not click the red axis to rotate the line tool.

..... Resizing the Line Tool

If you plan to generate a rake surface, you can resize the line tool to define the length of the rake.

Click the mouse-probe button in one of the white rectangles at the ends of the "line" part of the

tool (shown in black in Figure . : The Line Tool (p. )) and drag the mouse to lengthen or shorten

the tool. Green arrows will show the direction of stretching/shrinking.

..... Resetting the Line Tool

If you "lose" the line tool, or want to reset it for any other reason, you can either click Reset to return

the line tool to the default position and start from there, or turn the tool off and re-initialize it as

described above. In the default position, the line tool will lie midway along the  and  lengths of

the domain, spanning the  domain extent.

... Plane Surfaces

To display flow-field data on a specific plane in the domain, you will use a plane surface. You can

create surfaces that cut through the solution domain along arbitrary planes only in 3D; this feature is

not available in 2D.

There are six types of plane surfaces that you can create:

Intersection of the domain with the infinite plane:This is the default plane surface created.The extents of

the plane is determined by the extents of the domain. Because the plane is slicing through the domain,

the data points will, by default, be located where the plane intersects the faces of a cell, and consequently

may not be equally spaced.

Bounded plane:This plane will be a bounded parallelepiped, for which  of the  corners are the  points

that define the plane equation (or the  corners are the corners of the "plane tool"). Like the default plane

surface described above, this type of surface will also have unequally spaced data points.

Bounded plane with equally spaced data points:This plane is the same as the bounded plane described

above, except you will specify the density of points along the two directions of the parallelepiped, creating

a uniform distribution of data points.

Plane having a certain normal vector and passing through a specified point:To create this type of plane,

define a normal vector and a point. A plane with the specified normal and passing through the specified

point will be created.

Plane aligned with an existing surface:To create this type of plane, you will define a single point and a

surface. A plane parallel to the selected surface and passing through the specified point will be created.

Plane aligned with the view in the graphics window:To create this type of plane, you will define a single

point. A plane parallel to the current view in the active graphics window and passing through the specified

To create a plane surface, you will use the Plane Surface Dialog Box (p. ) (Figure . : The Plane

Domain → Surface → Create → Plane...

Figure . : The Plane Surface Dialog Box

The procedure for creating the plane surface is as follows:

.

Decide which of the six types of planes you want to create.

To create the default plane type (the intersection of the infinite plane with the domain), go directly

to step .

To create a bounded plane, select Bounded under Options.

To create a bounded plane with equally spaced data points, select both Bounded and Sample Points,

and then set the number of data points under Sample Density.You will specify the point density in

each direction by entering the appropriate values for Edge  and Edge . Edge  extends from point

to point , and edge  extends from point  to point .

To define a plane aligned with an existing surface, select Aligned With Surface, and then choose the

surface in the Surfaces list and specify a single point using one of the first two methods described

below in step .

To define a plane aligned with the view plane, select Aligned With View Plane, and then choose a

single point using one of the first two methods described below in step .

To define a plane having a certain normal vector and passing through a specified point, select Point

And Normal, and then specify the normal vector by entering values in the ix, iy, and iz fields under

Normal, and a single point using one of the first two methods described below in step .

.

Specify the location of the plane surface.There are three different ways to define the location:

Enter the coordinates of the three Points defining the planar surface: (x0, y0, z0), (x1, y1, z1), and

(x2, y2, z2).

Click Select Points and then select the three points by clicking on locations in the active graphics

window with the mouse-probe button. (See Controlling the Mouse Button Functions (p. ) for inform-

ation about setting mouse button functions.)

Use the Plane Tool option to interactively position a plane in the graphics window.You can set the

initial location of this plane using one of the two methods described above for specifying the defining

points.You can also start from the position defined by the default Points. See Using the Plane

Tool (p. ) for information about using the plane tool.

.

ID (for example, plane-). (If the New Surface Name you enter is the same as the name of a surface

Important

entry.

.

.... Using the Plane Tool

The plane tool enables you to interactively fine-tune the definition of a plane using graphics. Starting

from an initial plane, you can translate, rotate, and resize the plane until its position, orientation, and

size are as desired. For example, if you need to position a plane surface at a cross-section of an irreg-

ularly-shaped, curved duct, you can start with the plane tool near the desired location, resize it,

translate it until it is within the duct walls, and rotate it to the proper orientation. You may find it

helpful to display mesh faces to ensure that the plane tool is correctly positioned inside the domain.

..... Initializing the Plane Tool

Before enabling the Plane Tool option, set the Points to suitable starting values. You can enter

values manually, or use the Select Points button. Often it is convenient to display the mesh for an

inlet or isosurface that is similar to the desired plane surface, and then select three points on that

mesh to position the initial plane. Once you have specified the appropriate Points, enable the Plane

Tool option. The plane tool will appear in the graphics window, as shown in Figure . : The Plane

Tool (p. ).

Figure . : The Plane Tool

You can then translate, rotate, and/or resize the plane tool as described in the following sections.

.....Translating the Plane Tool

To translate the plane tool in the direction normal to the plane, click the mouse-probe button (the

right button by default) anywhere on the gray part of the plane tool and drag the mouse until the

about changing the mouse functions see Controlling the Mouse Button Functions (p. ).

To translate the tool in the transverse directions (that is, along either of the axes that lie within the

plane), press Shift, click the mouse-probe button anywhere on the gray part of the plane tool, and

drag the mouse until the tool reaches the desired location. Two sets of green arrows will show the

possible directions of motion. If you find the perspective distracting when performing this type of

translation, you can turn it off in the Camera Parameters Dialog Box (p. ) (opened from the Views

Dialog Box (p. )), as described in Controlling Perspective and Camera Parameters (p. ).

..... Rotating the Plane Tool

To rotate the plane tool, click the mouse-probe button on one of the white arrows at the tips of the

plane’s axes. Clicking on any arrow rotates the tool about either of the other two axes: when you

click the arrow, two green ribbons will encircle the plane tool, forming circles about each of the two

possible axes of rotation. Drag the mouse along the desired circle to rotate the tool. As you do so,

the circle along which the tool is rotating will become yellow.

The following notes may help you when you are rotating the plane tool:

Once you move your mouse along one circle, you cannot change the direction of rotation unless you

release the mouse-probe button and try again. Be careful to start moving your mouse very steadily so

that you can choose the correct direction.

Do not click the red arrow to rotate.

Do not try to rotate by clicking on an arrow that is pointing away from you. It will be very difficult for

you to judge which direction of rotation is correct from this point of view. Because there are two arrows

on each axis, there will always be an appropriate arrow available.

Do not rotate the plane tool more than ° or so at once. If you rotate the tool by a large angle, the arrow

on which you are clicking will begin to point away from you, and you will have trouble controlling the

rotation (as discussed in the item above).

..... Resizing the Plane Tool

If you plan to generate a bounded plane, you can resize the plane tool to define the plane’s

boundaries. Click the mouse-probe button in one of the white squares at the plane tool’s corners

(shown in black in Figure . : The Plane Tool (p. )) and drag the mouse to stretch or shrink the

tool. Green arrows will show the direction of the plane’s diagonal.

Important

Be careful not to drag your mouse across any of the axes while resizing the tool. This will

flip the tool over and corrupt it. If you accidentally do this, reset the plane tool and start

again.

..... Resetting the Plane Tool

If you "lose" the plane tool, or want to reset it for any other reason, you can either click Reset Points

to return the plane tool to the default position and start from there, or turn the tool off and re-ini-

tialize it as described above. In the default position, the plane tool will lie midway along the  length

of the domain, spanning the  and  domain extents.

... Quadric Surfaces

If you want to display data on a line (2D), plane (3D), circle (2D), sphere (3D), or general quadric surface,

you can specify the surface by entering the coefficients of the quadric function that defines it. This

feature provides you with an explicit method for defining surfaces. See Line and Rake Surfaces (p. )

and Plane Surfaces (p. ) for additional methods for creating line and plane surfaces.

To create a quadric surface, you will use the Quadric Surface Dialog Box (p. ) (Figure . : The

Quadric Surface Dialog Box (p. )).

Domain → Surface → Create → Quadric...

Figure . : The Quadric Surface Dialog Box

The steps for creating the quadric surface are as follows:

.

Decide which type of quadric surface you want to create. In 3D, choose Plane, Sphere, or (general)

Quadric in the Type drop-down list. In 2D, choose Line, Circle, or Quadric.

.

Specify the defining equation for the surface in SI units.

Line or plane surface: If you have selected Line (in 2D) or Plane (in 3D) as the surface type, the surface

will consist of all points on the domain that satisfy the equation

.You will

specify ix (the coefficient of ), iy (the coefficient of ), iz (the coefficient of ), and distance (the

distance of the line or plane from the origin) in the fields to the right of the Type drop-down list.When

you click Update under the Quadric Function heading, the display of the quadric function coefficients

will change to reflect your inputs.

Circle or sphere surface: If you have selected Circle (in 2D) or Sphere (in 3D) as the surface type, the

surface will consist of all points on the domain that satisfy the equation

.

You will specify x0, y0, z0 (the ,

, and  coordinates of the sphere or circle’s center) and r (the radius)

in the fields to the right of the Type drop-down list.When you click Update under the Quadric

Function heading, the display of the quadric function coefficients will change to reflect your inputs.

Quadric surface: If you have selected Quadric as the surface type, the surface will consist of all points

in the domain that satisfy the general quadric function

.You will specify the coefficients of

the quadric function  (the coefficients of the terms

,

,

, xy, yz, zx, x, y, z and the constant term)

directly in the Quadric Function box, and you will set value to the right of the Type drop-down list.

Note that the Update button will be disabled when you choose this type of surface.

.

ID (for example, sphere-slice- or quadric-slice-). If the New Surface Name you enter is

the same as the name of a surface that already exists, ANSYS Fluent will automatically assign the default

name to the new surface when it is created.

Important

entry.

.

Important

entry.

.

... Isosurfaces

If you want to display results on cells that have a constant value for a specified variable, you will need

to create an isosurface of that variable. Generating an isosurface based on ,

, or  coordinate, for

example, will give you an ,

, or  cross-section of your domain; generating an isosurface based on

pressure will enable you to display data for another variable on a surface of constant pressure. You

can create an isosurface from an existing surface or from the entire domain. Furthermore, you can restrict

any isosurface to a specified cell zone.

Important

Note that you cannot create an isosurface until you have initialized the solution, performed

calculations, or read a data file.

To create an isosurface, you will use the Iso-Surface Dialog Box (p. ) (Figure . : The Iso-Surface

Domain → Surface → Create → Iso-Surface...

Figure . : The Iso-Surface Dialog Box

The steps for creating the isosurface are as follows:

.

Choose the scalar variable to be used for isosurfacing in the Surface of Constant drop-down list. First,

select the desired category in the upper list.You can then select from related quantities from the lower

list. (See Field Function Definitions (p. ) for an explanation of the variables in the list.)

.

If you want to create an isosurface from an existing surface (that is, generate a new surface of constant

,

, temperature, pressure, and so on that is a subset of another surface), choose that surface in the

From Surface list.You can specify the cell zone on which you want to create an isosurface by selecting

the zone in the From Zones list.

If you do not select a surface from the list, the isosurfacing will be performed on the entire domain.

If you do not select a zone from the list, then the isosurfacing will not be restricted to any cell zone

and will run through the entire domain.

.

Click Compute to calculate the minimum and maximum values of the selected scalar field in the domain

or on the selected surface (in the From Surface list).The minimum and maximum values will be displayed

in the Min and Max fields.

.

Set the isovalue using one of the following methods. (Note that the second method will enable you to

define multiple isovalues in a single isosurface.)

You can set an isovalue interactively by moving the slider with the left mouse button.The value in

the Iso-Values field will be updated automatically.This method will also create a temporary isosurface

in the graphics window. Using the slider enables you to preview an isosurface before creating it.

Important

Even though the isosurface is displayed, it is only a temporary surface. To create an

isosurface, use the Create button after deciding on a particular isovalue.

You can type in isovalues in the Iso-Values field directly, separating multiple values by white space.

Multiple isovalues will be contained in a single isosurface; that is, you cannot select subsurfaces

within the resulting isosurface.

.

ID (for example, z-coordinate-). (If the New Surface Name you enter is the same as the name of

Important

entry.

.

Click Create.The new surface name will be added to the From Surface list in the dialog box.

... Clipping Surfaces

If you have created a surface, but you do not want to use the whole surface to display data, you can

clip the surface between two isovalues to create a new surface that spans a specified subrange of a

specified scalar quantity. The clipped surface consists of those points on the selected surface where

the scalar field values are within the specified range. For example, in Figure . : External Wall Surface

Isoclipped to Values of x Coordinate (p. ) the external wall has been clipped to values of  coordinate

less than  to show only the back half of the wall, enabling you to see the valve inside the intake port.

Figure . : External Wall Surface Isoclipped to Values of x Coordinate

To clip an existing surface, you will use the Iso-Clip Dialog Box (p. ) (Figure . : The Iso-Clip Dialog

Box (p. )).

Domain → Surface → Create → Iso-Clip...

Figure . : The Iso-Clip Dialog Box

The steps for clipping a surface are as follows:

. Choose the scalar variable on which the clipping will be based in the Clip To Values Of drop-down list.

First, select the desired category in the upper list.You can then select from related quantities from the

lower list. See Field Function Definitions (p. ) for an explanation of the variables in the list.

. Select the surface to be clipped in the Clip Surface list.

. Click Compute to calculate the minimum and maximum values of the selected scalar field on the selected

surface.The minimum and maximum values are displayed in the Min and Max fields.

. Define the clipping range using one of the following methods.

You can set the upper and lower limits of the clipping range interactively by moving the indicator in

each dial (that is, the dial above the Min or Max field) with the left mouse button.The value in the

corresponding Min or Max field is updated automatically.This method will also create a temporary

surface in the graphics window. Using the dials enables you to preview a clipped surface before creating

it.

Important

Even though the clipped surface is displayed, it is only a temporary surface. To create

it.

Important

the new surface, use the Clip button after deciding on the clipping range.

You can type the minimum and maximum values in the clipping range directly in the Min and Max

fields.

. If you do not want to use the default name assigned to the surface, enter a new name under New Surface

ID (for example, clip-density-). (If the New Surface Name you enter is the same as the name of a

surface that already exists, ANSYS Fluent will automatically assign the default name to the new surface

Important

The surface name that you enter must begin with an alphabetical letter. If the name of

the surface begins with any other character or number, ANSYS Fluent rejects the entry.

. Click Clip.The new surface name is added to the Clip Surface list in the dialog box. (The original surface

will remain unchanged.)

...Transforming Surfaces

You can create a new data surface from an existing surface by rotating and/or translating the original

surface. For example, you can rotate the surface of a complicated turbomachinery blade to plot data

in the region between blades. You can also create a new surface at a constant normal distance from

the original surface.

To transform an existing surface to create a new one, you will use the Transform Surface Dialog

Box (p. ) (Figure . : The Transform Surface Dialog Box (p. )).

Domain → Surface → Create → Transform...

Figure . : The Transform Surface Dialog Box

The steps for transforming a surface are as follows:

. Select the surface to be transformed in the Transform Surface list.

Important

The transform operation is not available for user-created surfaces such as lines, points,

iso-surfaces, and so on. To create a transformed line, point, iso-surface, or other user-

created surface, you must manually translate the input point(s) and create a new

line/point/iso-surface in the respective dialog box (Line/Rake, Point Surface, Iso-Surface,

and so on).

. Set the appropriate transformation parameters, as described below.You can perform any combination

of translation, rotation, and “isodistancing” on the surface.

Rotation:To rotate a surface, specify the origin about which the surface is rotated, and the angle by

which the surface is rotated.

In the About box under Rotate, specify a point, and the origin of the coordinate system for the

rotation will be set to that point. (The ,

, and  directions will be the same as for the global

coordinate system.) For example, if you specified the point (,,) in 3D, rotation would be about

the ,

, and  axes anchored at (,,). You can either enter the point’s coordinates in the x,

y, and z fields or click Mouse Select and select a point in the graphics window using the mouse-

probe button. See Controlling the Mouse Button Functions (p. ) for information about mouse

button functions.

In the Angles box under Rotate, specify the angles about the ,

, and  axes (that is, the axes

of the coordinate system with the origin defined under About) by which the surface is rotated.

For 2D problems, you can specify rotation about the  axis only.

Translation:To translate a surface, define the distance by which the surface is translated in each direction.

Set the x, y, and z translation distances under Translate.

Isodistancing:To create a surface positioned at a constant normal distance around the original surface,

set the value for d under Iso-Distance.

ID (for example, transform-). If the New Surface Name you enter is the same as the name of a surface

is created.

Important

. Click Create.The new surface name is added to the Transform Surface list in the dialog box.The original

surface will remain unchanged.

... Grouping, Editing, Renaming, and Deleting Surfaces

Once you have created a number of surfaces, you can edit, rename, delete, and group surfaces and

obtain information about their components. Grouping surfaces is useful if you want to perform post-

processing on a number of surfaces at a time. For example, you may want to group several wall surfaces

together to generate a contour plot of temperature on all walls. To postprocess results on each wall

surface individually,“ungroup” the surfaces.

You can manipulate existing surfaces and create new ones through the Surfaces branch of the Outline

View.

Additionally, you can manipulate existing surfaces within the Surfaces Dialog Box (p. ) (Fig-

ure . : The Surfaces Dialog Box (p. )).

Domain → Surface → Manage...

Figure . : The Surfaces Dialog Box

You can also open this dialog box by clicking Manage... in one of the surface creation dialog boxes

described in the previous sections or by double-clicking the Surfaces branch in the Outline View.

.... Grouping Surfaces

.... Editing and Renaming Surfaces

.... Deleting Surfaces

.... Surface Statistics

As mentioned above, you may want to group several surfaces together in order to perform postpro-

cessing on all of them at once. To create a surface group, select the surfaces to be grouped in the

Surfaces list. You can define a new name for the group in the Name field, or you can use the default

name, which is the name of the first surface you selected in the Surfaces list. Then click Group. The

selected surfaces disappear from the Surfaces list, and the name of the surface group is added to

the list.

Important

The Group button will not appear until you have selected at least two surfaces. As soon

as you choose a second surface in the Surfaces list, the Rename button will change to

the Group button.

To ungroup the surfaces, simply select the surface group in the Surfaces list and click UnGroup. The

group name will disappear from the list and the names of the original surfaces in the group will re-

appear in the list.

You can edit surfaces either by double-clicking the surface in the Surfaces branch of the Outline

View or by right-clicking it and selecting Edit.... This opens the respective surface dialog box where you

can modify settings and rename the surface.

<surface-name> → Edit...

To change the name of an existing surface, select the surface in the Surfaces list of the Surfaces

dialog box, enter a new name in the Name field, and then click Rename. The new name replaces the

old name in the Surfaces list and the surface is otherwise unchanged.

If you select more than one surface, the Rename button will not appear in the dialog box. When

more than one surface is selected, the Rename button is replaced by the Group button.

Important

If you find that a surface is no longer useful, you may want to delete it to prevent the list of surfaces

from becoming too cluttered. Select the surface or surfaces to be deleted in the Surfaces list, and

then click Delete. The delete operation is not reversible, so if you want to get a deleted surface back

again you will need to recreate it using one of the surface-creation dialog boxes described in the

previous sections.

You can also use the Surfaces Dialog Box (p. ) to retrieve topological information about surfaces.

Points is the total number of nodes in a surface. 0D Facets is the number of isolated nodes in a

surface (that is, nodes that have no connectivity, such as point surfaces or nodes in a rake), 1D Facets

is the number of linear faces (consisting of two connected nodes) in a surface in a 2D problem, and

2D Facets is the number of 2D faces (triangular or quadrilateral) in a surface in a 3D problem. Note

that an interior zone surface in a 3D problem consists of 2D facets, and similarly an interior zone

surface in a 2D problem consists of 1D facets.

These statistics are listed for the surface(s) selected in the Surfaces list. If more than one surface is

selected, the sum over all selected surfaces is displayed for each quantity.

Note that if you want to check these statistics for a surface that was read from a case file, you will

need to first display it.

Cell registers are a means for marking cells based on certain criteria, such as iso-values or proximity to

a boundary. You can then use these marked cell registers to perform operations like refining or

coarsening the mesh (Adapting the Mesh (p. )) or patching the solution (Patching Values in Selected

Cells (p. )).

The following sections describe how to create and use cell registers:

... Region

... Boundary

...Variable Limiter

... Field Variable

... Residuals

...Volume

...Yplus/Ystar

... Manage Cell Registers

... Cell Register Operations

... Copying and Renaming Cell Registers

Note

If you have multiple cell registers that you want to display within the same graphics window,

you can enable the Overlays option in the Scene Description dialog box (accessed by clicking

Compose... in the View ribbon tab).With this option enabled, each subsequent cell register you

display is shown on top of the existing graphics window display.

(Parallel only) The exact number of cells in a register may vary between sessions running on dif-

ferent core counts for the same case. However, any cell count variations are not to a degree that

they could impact the results.

... Region

Region registers allow you to mark cells inside or outside of a given region that you can specify using

text or mouse inputs. Using text input, you can specify the region as a hexahedron (quadrilateral in

2D), a sphere (circle in 2D), or a cylinder.

.... Defining a Region

The basic approach to creating a region cell register is to first define a region:

The hexahedron (quadrilateral) is defined by entering the coordinates of two points defining the diagonal.

The sphere (circle) is defined by entering the coordinates of the center of the sphere and its radius.

To define a cylinder, specify the coordinates of the points defining the cylinder axis, and the radius. In 3D

this will define a cylinder. In 2D, you will have an arbitrarily oriented rectangle with length equal to the

cylinder axis length and width equal to the radius.

A rectangle defined using the cylinder option differs from one defined with the quadrilateral option

in that the former can be arbitrarily oriented in the domain, while the latter must be aligned with

the coordinate axes.

You can either enter the exact coordinates into the appropriate real entry fields or select the locations

with the mouse on displays of the mesh or solution field. After the region is defined, each cell that

has a centroid inside/outside the specified region is marked.

.... Setting Up a Region Cell Register

To create a region cell register:

. Open the Figure . : Region Register Dialog Box (p. ).

New → Region...

Using Cell Registers

Figure . : Region Register Dialog Box

. Specify whether the register includes cells Inside or Outside of the defined region.

If you choose Inside, cells with centroids within the specified region will be marked.

If you choose Outside, cells with centroids outside the specified region will be marked.

. Choose the shape for the region register.

In 2D, you may specify a Quad (that is, a quadrilateral), Circle, or Cylinder by making a selection

from the Shapes group box. In 3D, your options include Hex (that is, a hexahedron), Sphere, or

Cylinder.

. Define the region by entering values into the dialog box or by using the mouse.

In the dialog box, the inputs are as follows:

Cylinder.

To define a hexahedron or quadrilateral, enter the coordinates of two points defining the diagonal of

the box.

For a hexahedron, define X Min, Y Min, and Z Min, as well as X Max, Y Max, and Z Max. For a

quadrilateral, define X Min and Y Min, as well as X Max and Y Max.

To define a sphere or circle, enter the values for the Radius and the coordinates of its center: X Center,

Y Center, and Z Center for a sphere, or X Center and Y Center for a circle.

To define a cylinder, enter the value for the Radius and the minimum and maximum coordinates de-

fining the cylinder axis: X-Axis Min, Y-Axis Min, and Z-Axis Min, as well as X-Axis Max, Y-Axis Max,

and Z-Axis Max for 3D, or X-Axis Min and Y-Axis Min, as well as X-Axis Max and Y-Axis Max for 2D.

In 2D, this will be the width of the resulting rectangle.

To define the region using the mouse, click the Select Points with Mouse button. Using the right

mouse button, select the input coordinates from a display of the mesh or solution field. After se-

lecting the points, the values will be loaded automatically into the appropriate fields in the dialog

box. See Controlling the Mouse Button Functions (p. ) for details about mouse button functions.

You have the option of editing these values before marking .

To define a hexahedron or quadrilateral, select the two points of the diagonal in any order.

To define a sphere or circle, first select the location of the centroid and then select a point that lies on

the sphere/circle (that is, a point that is one radius away from the centroid).

To define a cylinder, first select the two points that define the cylinder axis and then select a point

that is one radius away from the axis.

. Click Save to create the cell register.

Note

You can change the way the register is displayed by using the Cell Register Display

Options Dialog Box (p. ) dialog box that opens by clicking Display Options....

Boundary registers allow you to mark cells within the proximity of a boundary. The proximity to the

boundary can be based on:

cell distance—the distance of a cell from the boundary is measured by the number of cells.

normal distance—the distance is based on the normal distance of a cell from the boundary (using the se-

lected units for length).

volume distance—the distance is based on a target boundary volume and growth factor.

Cells are marked based on the following equation:

(.)

where

is the cell volume,

is the specified boundary volume (Boundary Volume),

is

the exponential growth factor (Growth Factor), and  is the normal distance of the cell centroid

from the selected boundaries.

is the target volume for a cell.

To create a boundary cell register:

. Open the Figure . : Boundary Register Dialog Box (p. ).

New → Boundary...

Figure . : Boundary Register Dialog Box

. Choose whether the boundary register is based on Cell Distance, Normal Distance, or Volume Distance.

. Specify the Number of Cells, Distance Threshold, or Boundary Volume and Growth Factor, depending

on which distance method you selected in the previous step.

. Select the boundary zone(s) for the cell register.

Note

Limit registers allow you to mark the cells that have reached a solution limit while solving. These limits

can be viewed and modified in Figure . : The Solution Limits Dialog Box (p. ). For additional in-

formation on solution limits, see Setting Solution Limits (p. ).

To create a limit cell register:

. Open the Figure . : Limit Register Dialog Box (p. ).

New → Variable Limiter...

Figure . : Limit Register Dialog Box

. Select the variable for creating the cell register.

Note

Field variable registers allow you to mark cells based on the value of a field variable. Additionally, you

can specify if these field variable values are derived, and if so, whether it is via gradient or curvature.

You can also scale the values by the zonal or global average or maximum. You can mark cells based

on the minimum/maximum value of a field variable, inside or outside of a certain range of field variable

values, within a certain percentage of the minimum/maximum value of a field variable, or by the top

or low value.

.... Approaches For Deriving Field Values

There are three approaches for using the available physical features of the flow field to mark cells

available in ANSYS Fluent:

Gradient approach: In this approach, ANSYS Fluent multiplies the Euclidean norm of the gradient of the

selected solution variable by a characteristic length scale  [] (p. ). For example, the gradient function

in two dimensions has the following form:

(.)

where

is the error indicator,

is the cell area,  is the gradient volume weight, and

is

the Euclidean norm of the gradient of the desired field variable,

.

The default value of the gradient volume weight is unity, which corresponds to full volume

weighting. A value of zero will eliminate the volume weighting, and values between  and  will

use proportional weighting of the volume.

This approach is recommended for problems with strong shocks, for example, supersonic inviscid

flows.

Curvature approach:This is an equidistribution marking technique that multiplies the undivided Laplacian

of the selected solution variable by a characteristic length scale  [] (p. ).

For example, the gradient function in two dimensions has the following form:

(.)

where

is

the undivided Laplacian of the desired field variable ( ).

This approach is recommended for problems with smooth solutions.

Isovalue approach:This approach is not based on derivatives. Instead, the isovalues of the required field

variable , are used to control the marking.Therefore, the function is of the form:

(.)

where

is the error indicator. This approach is recommended for problems where derivatives are

not helpful. For example, if you want to mark the mesh where the reaction is taking place, you can

use the isovalues of the reaction rate and mark at high reaction rates. This approach also allows

you to customize the criteria for controlling the marking using custom field functions, user-defined

scalars, and so on

Any of the field variables available for contours display can be used in the marking cell gradients.

These scalar functions include both geometric and physical features of the numerical solution.

Therefore, in addition to traditional marking based on physical features, such as the velocity, you may

choose to mark to the cell volume field to reduce rapid variations in cell volume.

In addition to the standard (no normalization) approach available in ANSYS Fluent, four options are

available for normalization  [] (p. ):

Scale by Global Average, scales the values of

,

, or

by their average value in the domain, that is:

(.)

Scale by Zone Average scales the values of

,

, or

by their average value in each zone.

,

, or

therefore always returning a problem-independent range of [, ] for any variable used for marking, that

is:

(.)

Scale by Zone Maximum, scales the values of

,

, or

by their maximum value in each zone,

is:

(.)

,

, or

therefore always returning a problem-independent range of [, ] for any variable used for marking.

.... Setting Up a Field Variable Cell Register

To create a field variable cell register:

. Open the Figure . : Field Variable Register Dialog Box (p. ).

New → Field Variable...

Figure . : Field Variable Register Dialog Box

. Choose the Type of field variable register. Note that you can use Compute to calculate the minimum

and maximum values of the chosen field variable.Your options include:

Min/Max Value Cells

cells containing the minimum and maximum values of the specified field variable will be marked.

Cells in Range

cells with isovalues between Iso-Min and Iso-Max will be marked.

Cells Less Than

cells with values that are less than the specified threshold value will be marked.

Cells More Than

cells with values that are greater than the specified threshold value will be marked.

Cells Outside Range

cells with isovalues less than Iso-Min or greater than Iso-Max will be marked.

Top Value Cells

cells with values within the top 'n' percent will be marked.

Low Value Cells

cells with values within the lowest 'n' percent will be marked.

. Specify how the field variable values are derived in the Derivative Option drop-down.You can choose

from:

None

Gradient

Curvature

. Specify how the field variable values are scaled in the Scaling Option drop-down.You can choose from:

None

Scale by Global Average

Scale by Zone Average

Scale by Global Maximum

Scale by Zone Maximum

None

. Select the field variable for creating the cell register from the Field Values of drop-down lists. The name

of this field will change based on the selections you make for derivative and scaling options.

Note

Residual registers allow you to mark cells based on their residuals values. You can visualize the cells

with the highest residual values and know their location so that you can modify them as necessary.

To create a residual cell register:

. Open the Figure . : Residual Register Dialog Box (p. ).

New → Residuals...

Figure . : Residual Register Dialog Box

. Select the Equation(s) for creating the residual cell register.

. Specify the Threshold Percent for creating the residual cell register. Cells with residual values above this

threshold for the selected equations are marked.

Note

...Volume

Volume registers allow you to mark cells based on the volume of the cells, either the magnitude or

the change in volume.

....Volume Cell Register Approach

Marking the mesh based on volume magnitude is often used to identify large cells. The procedure is

to mark cells with a volume greater than the specified threshold volume.

Marking the mesh based on the change in cell volume is used to identify areas where you may want

to improve the smoothness of the mesh. The procedure is to mark any cell that has a volume change

greater than the specified threshold value. The volume change is computed by looping over the faces

and comparing the ratio of the cell neighbors to the face.

For example, in Figure . : Volume Change—Ratio of the Volumes of the Cells (p. ) the ratio of

V1/V2 and the ratio of V2/V1 is compared to the threshold value. If V2/V1 is greater than the threshold,

then C2 is marked.

Figure . : Volume Change—Ratio of the Volumes of the Cells

.... Setting Up a Volume Cell Register

To create a volume cell register:

. Open the Figure . :Volume Register Dialog Box (p. ).

New → Volume...

Figure . : Volume Register Dialog Box

. Choose whether the cell register is based on the maximum size of the cells (Magnitude) or the Change

in volume of the cells.

. Specify the Max Volume or Max Volume Change. Note that you can click Compute to compute the

minimum and maximum cell volumes.

Note

Yplus/Ystar registers allow you to mark cells based on their Yplus/Ystar values.

....Yplus/Ystar Approach

The approach is to compute

or

or

for boundary cells on the specified viscous wall zones, define

the minimum and maximum allowable

or

, and mark the appropriate cells. Cells with

or

values below the minimum allowable threshold will be marked, as will cells with

or

values above

the maximum allowable threshold.

Figure . : Airfoil Wall Cells Marked by Y+ Values (p. ) shows a mesh created to solve the flow

over an airfoil, where the bottom boundary of the mesh that is shown is the top surface of the airfoil.

After an initial solution, it was determined that

values of some of the cells on the top surface were

too large, and

was used to mark them.

Figure . : Airfoil Wall Cells Marked by Y+ Values

.... Setting up a Yplus/Ystar Cell Register

To create a Yplus/Ystar cell register:

. Open the Figure . :Yplus/Ystar Register Dialog Box (p. ).

New → Yplus/Ystar...

Figure . : Yplus/Ystar Register Dialog Box

. Choose whether the cell register is based on Yplus or Ystar values.

. Select the Wall Zones for the Yplus or Ystar calculations.

. Specify the minimum and maximum Yplus/Ystar values allowed. Note that clicking Compute calculates

the minimum and maximum Yplus/Ystar values.

Note

The Figure . : Manage Cell Registers Dialog Box (p. ) allows you to review the properties of the

currently defined cell registers. You can also use it to display and delete the selected cell register.

To manage cell registers:

. Open the Figure . : Manage Cell Registers Dialog Box (p. ).

Edit...

Figure . : Manage Cell Registers Dialog Box

. Select a cell register to: view its properties, display it, or delete it.

Once a cell register is defined, you can create a cell register operation to report the residual values of

the selected cell registers at the interval you specify.

To create a register report:

. Open the Figure . : Report Register Dialog Box (p. ).

Solution → Calculation Activities → Cell Register Operations

New Report...

Figure . : Report Register Dialog Box

Note that this dialog box is only available after you have defined a cell register.

. Select the cell register(s) you want included in the report.

. Specify the reporting Frequency.

. Specify the maximum number of cells to include in the report.

. Click Save to create the cell register report.

The Figure . : Manage Register Operations Dialog Box (p. ) allows you to view properties, create,

modify, and delete report registers.

Edit...

Figure . : Manage Register Operations Dialog Box

The procedures for copying a cell register is as follows:

. In the Outline View, right-click the name of a cell register that you want to copy (under Setup/Solu-

tion/Cell Registers) and select Copy... to open the corresponding register dialog box.

. Enter the new name in the Name field and click Save/Display.

A new register will be added under the Cell Registers branch in the Outline View.

This is useful if you want to create a cell register with similar properties.

To change the name of a register:

. In the Outline View, select the cell register you want to rename. It becomes highlighted.

. Click the highlighted name again or press F2 to enter the edit mode.

. Type the new name and click outside of the name field to save it.

This procedure is similar to changing file names in Windows Explorer.

Chapter : Displaying Graphics

Graphics tools available in ANSYS Fluent enable you to process the information contained in your CFD

solution and easily view the results. The following sections explain how to use these tools to examine

your solution. The procedure for saving picture files of graphics displays is described in Saving Picture

.. Basic Graphics Generation

.. Customizing the Graphics Display

.. Controlling the Mouse Button Functions

..Viewing the Application Window

.. Modifying the View

.. Advanced Scene Composition

.. Animating Graphics

.. Histogram and XY Plots

..Turbomachinery Postprocessing

.. Fast Fourier Transform (FFT) Postprocessing

In ANSYS Fluent, you can generate graphics displays showing meshes, contours, profiles, vectors, pathlines,

and scenes. Some graphics are generated using variables that are plotted directly from the ANSYS Flu-

ent data file once the file has been read. The variables listed in the data file depend on the models

active at the time the file is written. Variables that are required by the solver, based on the current

model settings, but are missing from the data file are set to their default values. For those missing

variables, one iteration should be performed in order to obtain the required values for generating the

plot. A complete list of variables stored in the data file is available in (xfile.h) and can be accessed

as stated in Data Sections (p. ). The following sections describe how to create these plots. (Generation

of histogram and XY plots is discussed in Histogram and XY Plots (p. ).)

Important

If your model includes a discrete phase, you can also display the particle trajectories, as de-

scribed in Displaying of Trajectories (p. ).

Note

There are two kinds of graphics objects—those whose settings are saved with the case file

for reuse during the simulation, and those that are not. Persistent graphics objects (saved

with the case file) are accessed by clicking New..., non-persistent objects are created by

clicking Edit.... For example, you can create a persistent contour plot by clicking Contours

and selecting New... in the Results ribbon tab (Graphics group box).

Results → Graphics → Contours → New...

This section discusses the following topics:

... Displaying the Mesh

... Displaying Contours and Profiles

... Displaying Vectors

... Displaying Pathlines

... Displaying a Scene

... Displaying Results on a Sweep Surface

... Hiding the Graphics Window Display

During the problem setup or when you are examining your solution, you may want to look at the

mesh associated with certain surfaces. You can do the following:

Display the outline of all or part of the domain, as shown in Figure . : Outline Display (p. ).

Figure . : Outline Display

Draw the mesh lines (edges), as shown in Figure . : Mesh Edge Display (p. ).

Displaying Graphics

Figure . : Mesh Edge Display

Draw the solid surfaces (filled meshes) for a 3D domain, as shown in Figure . : Mesh Face (Filled

Mesh) Display (p. ).

Figure . : Mesh Face (Filled Mesh) Display

Basic Graphics Generation

Draw the nodes on the domain surfaces, as shown in Figure . : Node Display (p. ).

Figure . : Node Display

Note

The Post Processing option for mesh display configuration is recommended when postpro-

cessing your results in ANSYS Fluent. This option is accessed by clicking

in the objects

toolbar or by entering dislay/set/mesh-display-configuration in the console.

For information about displaying the mesh on a surface that sweeps through the domain, see Displaying

Results on a Sweep Surface (p. ).

.... Generating Mesh or Outline Plots

You can draw the mesh or outline for all or part of your domain using the Mesh Display Dialog

Box (p. ) (Figure . : The Mesh Display Dialog Box (p. )).

Results → Graphics → Mesh

Edit...

Figure . : The Mesh Display Dialog Box

Edit...

The basic steps for generating a mesh or outline plot are as follows:

.

Choose the surfaces for which you want to display the mesh or outline in the Surfaces list.

If you want to select several surfaces of the same type, click

and select Surface Type under

Group By, which organizes the surfaces in a tree view that is grouped by surface type.

Another shortcut is to use the Filter Text entry box to filter the Surfaces list to show only the

surfaces that match the pattern you enter. For additional information on using the Filter Text

entry box, see Filter Text Entry Boxes (p. ).

.

Depending on what you want to draw, do one or more of the following:

To draw an outline of the selected surfaces (as in Figure . : Outline Display (p. )), select Edges

under Options and Outline under Edge Type. If you need more detail in the outline display of a

complex geometry, see the description of the Feature option, below.

To draw the mesh edges (as in Figure . : Mesh Edge Display (p. )), select Edges under Options

and All under Edge Type.

To generate a filled-mesh display (as in Figure . : Mesh Face (Filled Mesh) Display (p. )), select

Faces under Options.

To draw the nodes on the selected surfaces (as in Figure . : Node Display (p. )), select Nodes

under Options.

.

Set any of the mesh and outline display options described in the following section.

.

Click Display to draw the specified mesh or outline in the active graphics window.

To display filled meshes, with smoothly shaded display, enable lighting and select a lighting interpol-

.

ation method other than Flat in the Display Options Dialog Box (p. ) or the Lights Dialog Box (p. ).

If you display nodes, and you want to change the symbol representing the nodes, you can change

the Point Symbol in the Display Options Dialog Box (p. ). See Modifying the Rendering Op-

.... Mesh and Outline Display Options

The options mentioned in the procedure in the previous section include modifying the mesh colors,

adding the outline of important features to an outline display, drawing partition boundaries, and

shrinking the faces and/or cells in the display.

..... Modifying the Mesh Colors

ANSYS Fluent enables you to control the colors that are used to render the meshes for each zone

type or surface. This capability can help you to understand mesh plots quickly and easily. To modify

the colors, open the Mesh Colors Dialog Box (p. ) (Figure . : The Mesh Colors Dialog Box (p. ))

by clicking Colors... in the Mesh Display Dialog Box (p. ).

Figure . : The Mesh Colors Dialog Box

You can set colors individually for the meshes displayed on each surface, using the Scene Description

By default, the Color by Type option is turned on, enabling you to assign colors based on zone

type. To change the color used to draw the mesh for a particular zone type, select the zone type in

the Types list and then select the new color in the Colors list. You will see the effect of your change

when you next display the mesh. Note that the surface type in the Types list applies to all surface

meshes (that is, meshes that are drawn for surfaces created using the dialog boxes opened from the

Create button in the Surface group box of the  Domain ribbon tab) except zone surfaces.

If you prefer to use the colors ANSYS Fluent assigns by zone ID, then you can display the mesh using

the Color by ID option.

Note

By default, walls are colored by preference color, which indicates that the color of the

walls will change based on the Graphics Color Theme specified in Preferences (available

from the File ribbon tab). For example, if you change the color theme from Gray Gradient

to Black, the wall color will automatically change from black to white to maintain visibility

(when preference color is selected for walls).

..... Adding Features to an Outline Display

For closed 3D geometries such as cylinders, the standard outline display often will not show enough

detail to accurately depict the shape. This is because for each boundary, only those edges on the

“outside” of the geometry (that is, those that are used by only one face on the boundary) are drawn.

In Figure . : Standard Outline of Complex Duct (p. ), which shows the outline display for a

complicated duct geometry, only the inlet and outlet are visible.

Figure . : Standard Outline of Complex Duct

Figure . : Feature Outline of Complex Duct

You can capture additional features using the Feature option in the Mesh Display Dialog Box (p. ).

(See Figure . : Feature Outline of Complex Duct (p. ).) Enable Feature under Edge Type, and

then set the Feature Angle. With the default Feature Angle of , if the difference between the

normal directions of two adjacent faces is more than °, the edge between those faces will be

drawn. Decreasing the Feature Angle will result in more edge lines (that is, more detail) being added

to the outline display. The appropriate angle for your geometry will depend on its curvature and

complexity. You can modify the Feature Angle until you find the value that yields the best outline

display.

..... Drawing Partition Boundaries

If you have partitioned your mesh for parallel processing, you can add the display of partition

boundaries to the mesh display by turning on the Partitions option in the Mesh Display Dialog

Box (p. ).

..... Shrinking Faces and Cells in the Display

To distinguish individual faces or cells in the display, enlarge the space between adjacent faces or

cells by increasing the Shrink Factor in the Mesh Display Dialog Box (p. ). The default value of

zero produces a display in which the edges of adjacent faces or cells overlap. A value of  creates

the opposite extreme: each face or cell is represented by a point and there is considerable space

between each one. A small value such as . may be large enough to enable you to distinguish

one face or cell from its neighbor. Displays with different Shrink Factor values are shown in Fig-

ure . : Mesh Display with Shrink Factor =  (p. ) and Figure . : Mesh Display with Shrink

Factor = . (p. ). Click Display to see the effect of the change in Shrink Factor.

Figure . : Mesh Display with Shrink Factor =

Figure . : Mesh Display with Shrink Factor = .

.... Creating and Using Mesh Plot Definitions

You can create named mesh plot definitions and save them for later use. See Creating and Using

Contour Plot Definitions (p. ) for additional information on graphics object definitions.

The steps for creating and using mesh plot definitions are similar to the steps for Generating Mesh

or Outline Plots (p. ), with the addition of a field for naming the mesh plot definition.

ANSYS Fluent enables you to plot contour lines or profiles superimposed on the physical domain.

Contour lines are lines of constant magnitude for a selected variable (isotherms, isobars, and so on).

A profile plot draws these contours projected off the surface along a reference vector by an amount

proportional to the value of the plotted variable at each point on the surface. Sample plots are shown

in Figure . : Contours of Static Pressure (p. ) and Figure . : Profile Plot of y Velocity (p. ).

For information about displaying contours or profiles on a surface that sweeps through the domain,

see Displaying Results on a Sweep Surface (p. ).

Figure . : Contours of Static Pressure

Figure . : Profile Plot of y Velocity

.... Generating Contour and Profile Plots

You can plot contours or profiles using the Contours Dialog Box (p. ) (Figure . : The Contours

Edit...

The basic steps for generating a contour or profile plot are as follows:

.

Edit...

.

Select the variable or function to be contoured or profiled in the Contours of drop-down list. First select

the desired category in the upper list; you may then select a related quantity in the lower list. (See Field

Function Definitions (p. ) for an explanation of the variables in the list.)

.

Choose the surface or surfaces on which to draw the contours or profiles in the Surfaces list. For 2D

cases, if no surface is selected, contouring or profiling is done on the entire domain. For 3D cases, you

must always select at least one surface.

.

Specify the number of contours or profiles in the Levels field.The maximum number of levels allowed

is .

.

If you are generating a profile plot, enable the Draw Profiles option. In the resulting Profile Options

Dialog Box (p. ) (Figure . :The Profile Options Dialog Box (p. )) you will define the profiles.

Figure . : The Profile Options Dialog Box

a.

Set the “zero height” reference value for the profile (Reference Value) and the length scale factor

for projection (Scale Factor). Any point on the profile with a value equal to the Reference Value

will be plotted exactly on the defining surface.Values greater than the Reference Value will be

projected ahead of the surface (in the direction of Projection Dir.) and scaled by Scale Factor),

and values less than the Reference Value will be projected behind the surface and scaled.

These parameters can be used to create fuller profiles when you need to display the variation

in a variable that is small compared to the absolute value of the variable. Consider, for ex-

ample, the display of temperature profiles when the temperature range in the domain is

from  K to  K. The  K range in the temperature will be hard to detect when profiles

are drawn using the default scaling (which will be based on the absolute magnitude of

K). To create a fuller profile, you can set the Reference Value to  and the profile

Scaling Factor to  (for example) to magnify the display of the remaining  K range. In

subsequent display of the profiles, the reference value of  will be effectively subtracted

from the data before display so that the temperatures of  K will not be offset from the

baselines. The profiles will then reflect only the variation of temperature from  K.

b.

Set the direction in which profiles are projected (Projection Dir.). In 2D, for example, a contour

plot of pressure on the entire domain can be projected in the  direction to form a carpet plot, or

a contour plot of  velocity on a sequence of -coordinate slice lines can be projected in the

direction to form a series of velocity profiles (as shown in Figure . : Profile Plot of y Velo-

city (p. )).

c.

c.

Click Apply and close the Profile Options Dialog Box (p. ).

.

Set any of the contour and profile plot options described below.

.

Click Display to draw the specified contours or profiles in the active graphics window.

The resulting display will include the specified number of contours or profiles of the selected variable,

with the magnitude on each one determined by equally incrementing between the values shown in

the Min and Max fields.

.... Contour and Profile Plot Options

The options mentioned in the procedure above include drawing color-filled contours/profiles (instead

of the default line contours/profiles), specifying a range of values to be contoured or profiled, including

portions of the mesh in the contour or profile display, choosing node or cell values for display, and

storing the contour or profile plot settings.

..... Drawing Filled Contours or Profiles

Color-filled contour or profile plots show a contour or profile display containing a continuous color

display (see Figure . : Filled Contours of Static Pressure (p. )), instead of just drawing lines

representing specific values. Note that a color-filled profile display is often referred to as a “carpet

plot”. To generate a filled contour or profile plot, enable the Filled option in the Contours Dialog

Box (p. ) during step  in the previous section.

Figure . : Filled Contours of Static Pressure

To display smoothly shaded filled contours, you must enable lighting and select a lighting interpol-

ation method other than Flat in the Display Options Dialog Box (p. ) or the Lights Dialog

Box (p. ). You will not get smooth shading of filled contours if the Clip to Range option is turned

on. Smooth shading of filled profiles is not available.

Note

The Draw Profile option settings are not saved with the contour plot definition. Once

the dialog box is closed these options will revert to being disabled.

..... Specifying the Range of Magnitudes Displayed

By default, the minimum and maximum values contoured or profiled are set based on the range of

values in the entire domain. This means that the color scale will start at the smallest value in the

domain (shown in the Min field) and end at the largest value (shown in the Max field). If you are

plotting contours or profiles on a subset of the domain (that is, on a surface), your plot may cover

only the midrange of the color scale. For example, if blue corresponds to  and red corresponds to

, and the values on your surface range only from  to , your plot will contain mostly green contours

or profiles, since green is the color at the middle of the default color scale.

To focus in on a smaller range of values, so that blue corresponds to  and red to , manually reset the

range to be displayed.You can also use the minimum and maximum values on the selected sur-

faces—rather than in the entire domain—to determine the range. Another reason to manually set the

range is if you are interested only in certain values. For example, if you want to determine the region

where pressure exceeds a certain value, you can increase the minimum value for display so that the lower

pressure values are not displayed.

To manually set the contour/profile range, turn off the Auto Range option in the Contours Dialog

Box (p. ).The Min and Max fields will become editable, and you can enter the new range of values to

be displayed.

– To show the default range at any time, click Compute and the Min and Max fields will be updated.

– If you are drawing filled contours or profiles you can control whether or not values outside the pre-

scribed Min/ Max range are displayed.

To leave areas in which the value is outside the specified range empty (that is, draw no contours or profiles),

enable the Clip to Range option.This is the default setting. If you turn Clip to Range off, values below

the Min value will be colored with the lowest color on the color scale, and values above the Max value

will be colored with the highest color on the color scale. Figure . : Filled Contours with Clip to Range

On (p. ) and Figure . : Filled Contours with Clip to Range Off (p. ) show the results of enabling/dis-

abling the Clip to Range option.

To base the minimum and maximum values on the range of values on the selected surfaces, rather than

in the entire domain, turn off the Global Range option in the Contours Dialog Box (p. ).The Min and

Max values will be updated when you next click Compute or Display.

Figure . : Filled Contours with Clip to Range On

Figure . : Filled Contours with Clip to Range Off

Note

When Global Range is enabled, Fluent only computes and populates the range when:

. You click Compute.

. Auto Range is enabled.

Note

If Auto Range is disabled, the range will remain the same until you click Compute, even if

you select a new variable for display.

..... Including the Mesh in the Contour Plot

mesh in your contour or profile plot as spatial reference points. For example, you may want to show

the location of an inlet and an outlet along with the contours. This is accomplished by turning on

the Draw Mesh option in the Contours Dialog Box (p. ). The Mesh Display Dialog Box (p. ) will

appear automatically when you enable the Draw Mesh option, and you can set the mesh display

parameters there. When you click Display in the Contours Dialog Box (p. ), the mesh display, as

defined in the Mesh Display Dialog Box (p. ), will be included in the contour or profile plot.

Note

The Draw Mesh option settings are not saved with the contour plot definition. Once the

dialog box is closed these options will revert to being disabled.

To include the mesh with a contour plot that will be persisted with the case file, you can

create a mesh plot definition and include both the mesh and contour plots in a scene.

See Displaying a Scene (p. ) for more details.

..... Choosing Node or Cell Values

In ANSYS Fluent you can choose to display the computed cell-center values or values that have been

interpolated to the nodes. By default, the Node Values option is turned on, and the interpolated

values are displayed. For line contours or profiles, node values are always used. To display filled

contours or profiles and to display the cell values, turn off the Node Values option. Filled contours/pro-

files of node values will show a smooth gradation of color, while filled contours/profiles of cell values

may show sharp changes in color from one cell to the next.

For face-only functions (for example, Wall Shear Stress), the cell values that are displayed for

boundary zone surfaces will actually be the face values. This is only true in the case of boundary

zone surfaces created for postprocessing, where the actual cell values are used for the part of the

surface that lies in the interior. These face values are more accurate, as face-only functions are

computed on the faces and not on the cells. For more information about cell values, see Cell Val-

ues (p. ).

If you are plotting contours to show the effect of a porous medium or 2D fan boundary, to depict

a shock wave, or to show any other discontinuities or jumps in the plotted variable, you should use

cell values; if you use node values in such cases, the discontinuity will be smeared by the node av-

eraging for graphics and will not be shown clearly in the plot.

..... Storing Contour Plot Settings

For frequently used combinations of contour variables and options, you can store the information

needed to generate the contour plot as follows:

. In the Contours Dialog Box (p. ), specify a Setup number.

. Set up the desired information in the Contours Dialog Box (p. ).

. Click Display.

The settings for Options, Contours of, Min, Max, and Surfaces will be saved.

You can then change the Setup number to an unused value (that is, an ID for which no information

has been saved) and generate a different contour plot.

To generate a plot using the saved setup information:

. Change the Setup number back to the value for which you saved contour information.

You can save up to  different setups.

Important

Note that the number of contour Levels, the surfaces selected for display in the Mesh

Display Dialog Box (p. ) (when the Draw Mesh option is activated), and the settings

for profiles in the Profile Options Dialog Box (p. ) (when the Draw Profiles option is

activated) will not be saved in the Setup, nor will the Setup be saved in the case file.

.... Creating and Using Contour Plot Definitions

You can create named contour plot definitions and save them for later use. This could be useful for

demonstration purposes, scene creation, or for postprocessing the results of your simulation when

varying the settings between runs (to name a few examples).

The number of contour plot definitions is not limited.

To create a contour plot definition:

New...

. In the Contours Dialog Box (p. ), in the Contour Name text entry box, enter the name for your contour

plot definition (or accept the default name contour-id).

Important

Contour and vector plot definitions must have unique names.

. Set contour parameters and options.

The Draw Mesh and Draw Profile option settings are not saved with the contour plot definition.

Once the dialog box is closed these options will revert to being disabled.

The specified contour will be displayed in the active graphics window, and the new contour plot

definition with the name you have entered will appear in the tree under Contours.

Once the contour plot definition is created, you can perform the following actions using the right-

click menu commands:

Edit the existing contour plot definition.

Copy the contour plot definition.

When creating a copy of the existing contour, you can modify contour settings in the Contours

dialog box that will open.

Delete the selected contour plot definition.

Display the contour in the graphics window.

Add the selected contour to the plot in the graphics window.

Note that while Display replaces the current contents of the graphics window, Add to graphics

preserves the current graphics window contents.

Note

You can move the colormap of contour plot definitions by left-clicking and dragging it to the

desired location.The colormap can also be resized by dragging the corners of the box that

appears when you hover over the colormap. The colormap location is not saved with the contour

plot definition.

For 2D cases, Fluent automatically creates a new surface when you click Save/Display in the

Contours dialog box, if you have not selected any surfaces for display. New surfaces are only

created for fluid zones that do not already have a surface defined.

These commands are also available through the text user interface (display/objects).

You can draw vectors in the entire domain, or on selected surfaces. By default, one vector is drawn at

the center of each cell (or at the center of each facet of a data surface), with the length and color of

the arrows representing the velocity magnitude (Figure . : Velocity Vector Plot (p. )). The spacing,

size, and coloring of the arrows can be modified, along with several other vector plot settings. Velocity

vectors are the default, but you can also plot vector quantities other than velocity. Note that cell-center

values are always used for vector plots; you cannot plot node-averaged values.

For information about displaying vectors on a surface that sweeps through the domain, see Displaying

Figure . : Velocity Vector Plot

.... Generating Vector Plots

You can plot vectors using the Vectors Dialog Box (p. ) (Figure . : The Vectors Dialog Box (p. )).

Edit...

Figure . : The Vectors Dialog Box

The procedure for generating a vector plot is as follows:

.

In the Vectors of drop-down list, select the vector quantity to be plotted. By default, only velocity

and relative velocity are available, but you can create your own custom vectors as described in

Creating and Managing Custom Vectors (p. ). Additional vector options are available for adjoint

solver results, as described in Field Data (p. ).

.

In the Surfaces list, choose the surface(s) on which you want to display vectors. If you want to display

vectors on the entire domain, select none of the surfaces in the list.

.

Set any of the vector plot options as described in Vector Plot Options (p. ).

.

Click Display to draw the vectors in the active graphics window.

.... Displaying Relative Velocity Vectors

If you are solving your problem using one or more moving reference frames or moving meshes, you

will have the option to display either the absolute vectors or the relative vectors. If you select Velocity

(the default) in the Vectors of list, the vectors will be drawn based on the absolute, stationary reference

frame. If you select Relative Velocity, the vectors will be drawn based on the reference frame of the

Reference Zone in the Reference Values Task Page (p. ). See Setting the Reference Zone (p. )

for details. (If you are modeling a single moving reference frame, you need not specify the Reference

Zone; the vectors will be drawn based on the moving reference frame.)

....Vector Plot Options

The options mentioned in the procedure above include scaling the vector arrows, skipping the display

of some vectors, displaying vectors in the plane of the data surface, displaying fixed-length or fixed-

color vectors, displaying directional components of the vectors, specifying a range of values to be

displayed, coloring the vectors by a different scalar field, including portions of the mesh in the vector

display, and changing the style of the arrows or the scale of the arrowheads.

The most common options are set in the Vectors Dialog Box (p. ), and others are set in the Vector

Options Dialog Box (p. ) (Figure . : The Vector Options Dialog Box (p. )), which you can open

by clicking Vector Options... in the Vectors Dialog Box (p. ).

Figure . : The Vector Options Dialog Box

..... Scaling the Vectors

By default, vectors are scaled automatically so that the arrows overlap minimally when no vectors

are skipped. For instructions on thinning the vector display, see “Thinning” Pathlines (p. ). With

the Auto Scale option, you can modify the Scale factor (which is set to  by default) to increase or

decrease the vector scale from the default “auto scale”. The main advantage of autoscaling is that

the vector display with a scale factor of  will always be appropriate, regardless of the size of the

domain, giving you a better starting point for fine-tuning the vector scale.

If you turn off the Auto Scale option, the vectors will be drawn at their actual sizes scaled by the

scale factor (Scale, which is set to  by default). The “actual” size of a vector is the magnitude of the

vector variable (velocity, by default) at the point where it is drawn. A vector drawn at a point where

the velocity magnitude is  m/s is drawn  m long, whether the domain is . m or  m. You

can modify the vector scale by changing the value of Scale in the Vectors Dialog Box (p. ) until

the size of the vectors (that is, the actual size multiplied by Scale) is satisfactory.

..... Skipping Vectors

If your vector display is difficult to understand because there are too many arrows displayed, you

can “thin out” the vectors by changing the Skip value in the Vectors Dialog Box (p. ). By default,

Skip is set to , indicating that a vector will be drawn for each cell in the domain or for each face

on the selected surface (for example,

vectors). If you increase Skip to , every other vector will be

displayed, yielding

vectors. If you increase Skip to , every third vector will be displayed,

yielding

vectors, and so on. The order of faces on the selected surface (or cells in the domain)

will determine which vectors are skipped or drawn; therefore adaption will change the appearance

of the vector display when a nonzero Skip value is used.

..... Drawing Vectors in the Plane of the Surface

For some problems, you may be interested in visualizing velocity (or other vector) components that

are normal to the flow. These “secondary flow” components are usually much smaller than the

components in the flow direction and are difficult to see when the flow direction components are

also visible. To easily view the normal flow components, you can enable the In Plane option in the

Vector Options Dialog Box (p. ). When this option is on, ANSYS Fluent will display only the vector

components in the plane of the surface selected for display. If the selected surface is a cross-section

of the flow domain, you will be displaying the components normal to the flow.

Figure . : Velocity Vectors Generated Using the In Plane Option (p. ) shows velocity vectors

generated using the In Plane option. Note that these vectors have been translated outside the do-

main, as described in Transforming Geometric Objects in a Scene (p. ), so that they can be seen

Figure . : Velocity Vectors Generated Using the In Plane Option

..... Displaying Fixed-Length Vectors

By default, the length of a vector is proportional to its velocity magnitude. If you want all of the

vectors to be displayed with the same length, you can enable the Fixed Length option in the Vector

Options Dialog Box (p. ). To modify the vector length, adjust the value of the Scale factor in the

Vectors Dialog Box (p. ).

..... Displaying Vector Components

All Cartesian components of the vectors are drawn by default, so that the arrow points along the

resultant vector in physical space. However, sometimes one of the components, say, the  component,

is relatively large. In such cases, you may want to suppress the  component and scale up the vectors,

in order to visualize the smaller  and  components. To suppress one or more of the vector com-

ponents, turn off the appropriate button(s) (X, Y, or Z Component) in the Vector Options Dialog

Box (p. ).

By default, the minimum and maximum vectors included in the vector display are set based on the

range of vector-variable (velocity, by default) magnitudes in the entire domain. If you want to focus

in on a smaller range of values, you can restrict the range to be displayed. The color scale for the

vector display will change to reflect the new range of values. (You can also use the minimum and

maximum values on the selected surfaces—rather than on the entire domain—to determine the

range, or change the scalar field by which the vectors are colored from velocity magnitude to any

other scalar, as described below.)

To manually set the range of velocity magnitudes (or the range of whatever scalar field is selected

in the Color by drop-down list), turn off the Auto Range option in the Vectors Dialog Box (p. ).

The Min and Max fields will become editable, and you can enter the new range of values to be

displayed. For example, if you want to display velocity vectors only in regions where the velocity

magnitude exceeds  m/s but is less than  m/s, you will change the value of Min to  and

the value of Max to . Similarly, if you are coloring the vectors by static pressure, you can choose

to display velocity vectors only in regions where the pressure is within a specified range. To show

the default range at any time, click Compute and the Min and Max fields will be updated.

When you restrict the range of vectors displayed, you can also control whether or not values outside

the prescribed Min/ Max range are displayed. To leave areas in which the value is outside the specified

range empty (that is, draw no vectors), enable the Clip to Range option. This is the default setting.

If you turn Clip to Range off, values below the Min value will be colored with the lowest color on

the color scale, and values above the Max value will be colored with the highest color on the color

scale. This feature is the same as the one available for displaying filled contours (see Figure . : Filled

Contours with Clip to Range On (p. ) and Figure . : Filled Contours with Clip to Range

Off (p. )).

You can also choose to base the minimum and maximum values on the range of values on the se-

lected surfaces, rather than the entire domain. To do this, turn off the Global Range option in the

Vectors Dialog Box (p. ). The Min and Max values will be updated when you next click Compute

or Display.

..... Changing the Scalar Field Used for Coloring the Vectors

If you want to color the vectors by a scalar field other than velocity magnitude (the default), you

can select a different variable or function in the Color by drop-down list. Select the desired category

in the upper list, and then choose one of the related quantities from the lower list. If you choose

static pressure, for example, the length of the vectors will still correspond to the velocity magnitude,

but the color of the vectors will correspond to the value of pressure at each point where a vector

is drawn.

..... Displaying Vectors Using a Single Color

If you want all of the vectors to be the same color, you can select the color to be used in the Color

drop-down list in the Vector Options Dialog Box (p. ). If no color is selected (that is, if you choose

the empty space at the top of the drop-down list—the default selection), the vector color will be

determined by the Color by field specified in the Vectors Dialog Box (p. ). Single color vectors

are useful in displays that overlay contours and vectors.

..... Including the Mesh in the Vector Plot

mesh in your vector plot as spatial reference points. For example, you may want to show the location

of an inlet and an outlet along with the vectors. This is accomplished by turning on the Draw Mesh

option in the Vectors Dialog Box (p. ). The Mesh Display Dialog Box (p. ) will appear automat-

ically when you enable the Draw Mesh option, and you can set the mesh display parameters there.

When you click Display in the Vectors Dialog Box (p. ), the mesh display, as defined in the Mesh

Display Dialog Box (p. ), will be included in the vector plot.

Note

The Draw Mesh option settings are not saved with the vector plot definition. Once the

dialog box is closed these settings will revert to being disabled.

To include the mesh with a vector plot that will be persisted with the case file, you can

create a mesh plot definition and include both the mesh and vector plots in a scene. See

Displaying a Scene (p. ) for more details.

..... Changing the Arrow Characteristics

There are seven different vector arrow styles available. Choose 3d arrow, 3d arrowhead, cone,

filled-arrow, arrow, harpoon, or headless in the Style drop-down list in the Vectors Dialog

Box (p. ).

If you choose a vector arrow style that includes heads, you can control the size of the arrowhead

by modifying the Scale Head value in the Vector Options Dialog Box (p. ).

.... Creating and Managing Custom Vectors

In addition to the velocity vector quantity provided by ANSYS Fluent, you can also define your own

custom vectors to be plotted. This capability is available with the Custom Vectors Dialog Box (p. ).

Any custom vectors that you define will be saved in the case file the next time that you save it. You

can also save your custom vectors to a separate file, so that they can be used with a different case

file.

..... Creating Custom Vectors

To create your own custom vector, you will use the Custom Vectors Dialog Box (p. ) (Fig-

ure . : The Custom Vectors Dialog Box (p. )). This dialog box enables you to define custom

vectors based on existing quantities. Any vectors that you define will be added to the Vectors of

list in the Vectors Dialog Box (p. ).

To open the Custom Vectors Dialog Box (p. ), click Custom Vectors... in the Vectors Dialog

Box (p. ).

Figure . : The Custom Vectors Dialog Box

The steps for creating a custom vector are as follows:

.

Specify the name of the custom vector in the Vector Name field.

Important

Do not specify a name that is already used for a standard vector (for example, velo-

city or relative-velocity).

.

Select the variable or function for the x component of the vector in the X Component drop-down list.

First select the desired category in the upper list; you may then select a related quantity in the lower

list. For an explanation of the variables in the list, see Field Function Definitions (p. ).

.

Repeat the step above to select the variable or function for the  component (and, in 3D, the  com-

ponent) of the custom vector.

Important

.

Important

You can use the Custom Vectors option to plot vectors in solid cell zones. The

scalars that are selected in the x, y (and, in 3D, the z) components, and that are valid

in solid regions, will have vector plots displayed in the solid cell zones. Note that if

a vector has no valid components in the solid region, then that vector will not be

plotted in the solid region. However, if at least one component of the vector is valid

in the solid region, then only that component of the vector will be plotted.

.

Click Define.

..... Manipulating, Saving, and Loading Custom Vectors

Once you have defined your vectors, you can manipulate them using the Vector Definitions Dialog

Box (p. ) (Figure . : The Vector Definitions Dialog Box (p. )). You can display a vector definition

to be sure that it is correct, delete the vector if you decide that it is incorrect and must be redefined,

or give the vector a new name. You can also save custom vectors to a file or read them from a file.

The custom vector file enables you to transfer custom vectors between case files.

To open the Vector Definitions Dialog Box (p. ), click Manage... in the Custom Vectors Dialog

Box (p. ).

Figure . : The Vector Definitions Dialog Box

The following actions can be performed in the Vector Definitions Dialog Box (p. ):

To check the definition of a vector, select it in the Vectors list. Its definition will be displayed in the X

Component, Y Component, and Z Component fields at the top of the dialog box.This display is for in-

formational purposes only; you cannot edit it. If you want to change a vector definition, you must delete

the vector and define it again in the Custom Vectors Dialog Box (p. ).

To delete a vector, select it in the Vectors list and click Delete.

To rename a vector, select it in the Vectors list, enter a new name in the Name field, and click Rename.

Important

To save all the vectors in the Vectors list to a file, click Save... and specify the file name in The Select File

To read custom vectors from a file that you saved as described above, click Load and specify the file

name in The Select File Dialog Box (p. ). (Custom vectors are valid Scheme functions, and can also be

loaded with the File/Read/Scheme... ribbon tab item, as described in Reading Scheme Source Files (p. ).)

.... Creating and Using Vector Plot Definitions

You can create named vector plot definitions and save them for later use. See Creating and Using

Contour Plot Definitions (p. ) for additional information on plot definitions.

The steps for creating and using vector plot definitions are similar to the steps for Generating Vector

Plots (p. ), with the addition of a field for naming the vector plot definition.

Note

You can move the colormap of a vector plot definition by left-clicking and dragging it to

the desired location. The colormap can also be resized by dragging the corners of the box

that appears when you hover over the colormap. The colormap location is not saved with

the vector plot definition.

Pathlines are used to visualize the flow of massless particles in the problem domain. The particles are

released from one or more surfaces that you have created by clicking Create in the Surface group

box of the  Domain ribbon tab (see Creating Surfaces and Cell Registers for Displaying and Reporting

Data (p. )). A line or rake surface (see Line and Rake Surfaces (p. )) is most commonly used. Fig-

ure . : Pathline Plot (p. ) shows a sample plot of pathlines.

Figure . : Pathline Plot

Note that the display of discrete-phase particle trajectories is discussed in Displaying of Trajector-

ies (p. ).

.... Steps for Generating Pathlines

You can plot pathlines using the Pathlines Dialog Box (p. ) (Figure . : The Pathlines Dialog

Box (p. )).

Results → Graphics → Pathlines

Edit...

Figure . : The Pathlines Dialog Box

The basic steps for generating pathlines are as follows:

.

Select the surface(s) from which to release the particles in the Release From Surfaces list.

.

(Eulerian Multiphase model only) From the Track in Phase drop-down list, select the phase in which

pathlines will be tracked. If you want to track pathlines in the mixture of all phases, select all-phase.

By default, particles are tracked in the primary phase.

.

Set the step size and the maximum number of steps.The Step Size sets the length interval used for

computing the next position of a particle. Note that particle positions are always computed when

particles enter/leave a cell; even if you specify a very large step size, the particle positions at the entry/exit

of each cell will still be computed and displayed.The value of Steps sets the maximum number of steps

a particle can advance. A particle will stop when it has traveled this number of steps or when it leaves

the domain. One simple rule of thumb to follow when setting these two parameters is that if you want

the particles to advance through a domain of length , the Step Size times the number of Steps should

be approximately equal to .

.

Set any of the pathline plot options described in Options for Pathline Plots (p. ).

.

Click Display to draw the pathlines, or click Pulse to animate the particle positions.The Pulse button

will become the Stop ! button during the animation, and you must click Stop ! to stop the pulsing.

.... Options for Pathline Plots

You can include the mesh in the pathline display, control the style of the pathlines (including the

twisting of ribbon-style pathlines), and color them by different scalar fields and control the color scale.

You can also “thin” the pathline display, trace the particle positions in reverse, and draw “oil-flow”

pathlines. If you are “pulsing” the pathlines, you can control the pulse mode. If you are using larger

time step size for calculations then you can control the accuracy of the pathline by specifying tolerance.

In addition to the regular pathline display, you can also generate an XY plot of a specified quantity

along the pathline trajectories. Finally, you can choose node or cell values for display (or plotting).

..... Including the Mesh in the Pathline Display

mesh in your pathline display as spatial reference points. For example, you may want to show the

location of an inlet and an outlet along with the pathlines (as in Figure . : Pathline Plot (p. )).

This is accomplished by turning on the Draw Mesh option in the Pathlines Dialog Box (p. ). The

Mesh Display Dialog Box (p. ) will appear when you enable the Draw Mesh option, where you

can set the mesh display parameters. When you click Display in the Pathlines Dialog Box (p. ),

the mesh display, as defined in the Mesh Display Dialog Box (p. ), will be included in the plot of

pathlines.

Note

The Draw Mesh option settings are not saved with the pathline definition. Once the

dialog box is closed these settings will revert to being disabled. If you want these settings

persisted within the current session, you can use the non-persistent Pathlines dialog box.

Results → Graphics → Pathlines → Edit...

..... Controlling the Pathline Style

Pathlines can be displayed as lines (with or without arrows), ribbons, cylinders (coarse, medium, or

fine), triangles, spheres, or a set of points. You can choose line, line-arrows, point, sphere, ribbon,

triangle, coarse-cylinder, medium-cylinder, or fine-cylinder in the Style drop-down list in the

Pathlines Dialog Box (p. ). Pulsing can be done only on point, sphere, or line styles.

Once you have selected the pathline style, click Style Attributes... to set the pathline thickness and

other parameters related to the selected Style:

If you are using the line or line-arrows style, set the Line Width in the Path Style Attributes Dialog

Box (p. ) that appears when you click Style Attributes.... For line-arrows you will also set the Spacing

Factor, which controls the spacing between the lines.The size of the arrow heads can be adjusted by

entering a value in the Scale text-entry box.

If you are using the point style, you will set the Marker Size in the Path Style Attributes Dialog Box (p. ).

The thickness of the pathline will be the thickness of the marker.

If you are using the sphere style, you will set the Diameter and the Detail in the Path Style Attributes

The best diameter to use will depend on the dimensions of the domain, the view, and the particle

density. However, an adequate starting point would be a diameter on the order of / of the av-

erage cell size or / step size. Units for the Diameter field correspond to the mesh dimensional

units.

Detail field in the Path Style Attributes Dialog Box (p. ). The level of detail uses integer values

ranging from  to . Note that the performance of the graphical rendering will be better when

using a small level of detail, that is, very coarse spheres, such as  or . The rendering performance

significantly decreases with higher levels of detail. You should gradually increase the detail to

determine the best-case scenario between performance and quality.

If you are using the triangle or any of the cylinder styles, you will set the Width in the Path Style Attributes

Dialog Box (p. ). For triangles, the specified value will be half the width of the triangle’s base, and for

cylinders, the value will be the cylinder’s radius.

If you are using the ribbon style, clicking Style Attributes... opens the Ribbon Attributes Dialog

Box (p. ), in which you can set the ribbon’s Width.You can also specify parameters for twisting the

ribbon pathlines. In the Twist By drop-down list, you can select a scalar field on which the pathline

twisting is based (for example, helicity). Select the desired category in the upper list and then select a

related quantity in the lower list.The twisting may not be displayed smoothly because the scalar field

by which you are twisting the pathline is calculated at cell centers only (and not interpolated to a particle’s

position).The Twist Scale sets the amount of twist for the selected scalar field.To magnify the twist for

a field with very little change, increase this factor; to display less twist for a field with dramatic changes,

decrease this factor.

..... Controlling Pathline Colors

By default, the pathlines are colored by the particle ID number. That is, each particle’s path will be

a different color. You can also choose the color based on the surface from where the pathlines were

released from using the surface ID as the particle variable. You can choose to color the pathlines by

any of the scalar fields in the Color by drop-down list. Select the desired category in the upper list

and then select a related quantity in the lower list. If you color the pathlines by velocity magnitude,

for example, each particle’s path will be colored depending on the speed of the particle at each

point in the path.

The range of values of the selected scalar field will, by default, be the upper and lower limits of that

field in the entire domain. The color scale will map to these values accordingly. If you prefer to restrict

the range of the scalar field, turn off the Auto Range option (under Options) and set the Min and

Max values manually beneath the Color by list. If you color the pathlines by velocity, and you limit

the range to values between  and  m/s, for example, the “lowest” color will be used when the

particle speed falls below  m/s and the “highest” color will be used when the particle speed exceeds

m/s. To show the default range at any time, click Compute and the Min and Max fields will be

updated.

.....“Thinning” Pathlines

If your pathline plot is difficult to understand because there are too many paths displayed, you can

“thin out” the pathlines by changing the Path Skip value in the Pathlines Dialog Box (p. ). By

default, Path Skip is set to , indicating that a pathline will be drawn from each face on the selected

surface (for example,

pathlines). If you increase Path Skip to , every other pathline will be displayed,

yielding

pathlines. If you increase Path Skip to , every third pathline will be displayed, yielding

yielding

, and so on. The order of faces on the selected surface will determine which pathlines are skipped

or drawn; therefore adaption will change the appearance of the pathline display when a nonzero

Path Skip value is used.

..... Coarsening Pathlines

To further simplify pathline plots, and reduce plotting time, a coarsening factor can be used to reduce

the number of points that are plotted. Providing a coarsening factor of , will result in each

th

point being plotted for a given pathline in any cell. This coarsening factor is specified in the Pathlines

Dialog Box (p. ), in the Path Coarsen field. For example, if the coarsening factor is set to , then

ANSYS Fluent will plot alternate points.

Important

..... Reversing the Pathlines

If you are interested in determining the source of a particle for which you know the final destination

(for example, a particle that leaves the domain through an exit boundary), you can reverse the

pathlines and follow them from their destination back to their source. To do this, enable the Reverse

option in the Pathlines Dialog Box (p. ). All other inputs for defining the pathlines will be exactly

the same as for forward pathlines; the only difference is that the surface(s) selected in the Release

From Surfaces list will be the final destination of the particles instead of their source.

..... Plotting Oil-Flow Pathlines

If you want to display “oil-flow” pathlines (that is, pathlines that are constrained to lie on a particular

boundary), enable the Oil Flow option in the Pathlines Dialog Box (p. ). You will then need to

select a single boundary zone in the On Zone list. The selected zone is the boundary on which the

oil-flow pathlines will lie.

..... Controlling the Pulse Mode

If you are going to use the Pulse button in the Pathlines Dialog Box (p. ) to animate the pathlines,

you can choose one of two pulse modes for the release of particles that follow the pathlines. To release

a single wave of particles, select the Single option under Pulse Mode. To release particles continu-

ously from the initial positions, select the Continuous option.

..... Controlling the Accuracy

If you are using large time step size for the calculation, there might be significant error introduced

while calculating the pathlines. To control this error, select Accuracy Control and specify the value

of Tolerance. The tolerance value will be taken in to consideration while calculating the pathlines

for each time step.

..... Plotting Relative Pathlines

If you want to display the pathlines relative to the moving reference frame, enable the Relative

Pathlines option in the Pathlines Dialog Box (p. ). You will then need to select the surfaces from

the Release from Surfaces list.

..... Generating an XY Plot Along Pathline Trajectories

If you want to generate an XY plot along the trajectories of the pathlines you have defined, enable

the XY Plot option in the Pathlines Dialog Box (p. ). The Color by drop-down list will be replaced

by Y Axis Function and X Axis Function lists. Select the variable to be plotted on the -axis in the

Y Axis Function list, and specify whether you want to plot this quantity as a function of the Time

elapsed along the trajectory, or the Path Length along the trajectory by selecting the appropriate

item in the X Axis Function drop-down list. Specify the Step Size, number of Steps, and other

parameters as usual for a standard pathline display. Then click Plot to display the XY plot.

Once you have generated an XY plot, you may want to save the plot data to a file. You can read

this file into ANSYS Fluent at a later time and plot it alone using the File XY Plot Dialog Box (p. ),

as described in XY Plots of File Data (p. ), or add it to a plot of solution data, as described in In-

cluding External Data in the Solution XY Plot (p. ).

To save the plot data to a file, enable the Write to File option in the Pathlines Dialog Box (p. ).

The Plot button changes to a Write... button. Clicking Write... opens The Select File Dialog Box (p. ),

in which you can specify a name and save a file containing the plot data. The format of this file is

described in XY Plot File Format (p. ).

..... Saving Pathline Data

To save pathline data to a file, perform the following steps:

.

Enable the Write to File option in the Pathlines Dialog Box (p. ) (Figure . :The Pathlines Dialog

Box (p. )).

.

In the Type drop-down list, select one of the following types of files:

Standard for FIELDVIEW (.fvp) format

Geometry for .ibl format (which can be read by GAMBIT)

EnSight format

Important

If you plan to write the pathline data in EnSight format, you should first verify that

you have already written the files associated with the EnSight Case Gold file type

Important

by using the File/Export... ribbon tab option (see EnSight Case Gold Files (p. )).

For further information about the files that are written for any of these types, refer to the appro-

priate section following these steps.

.

Choose to color the pathlines by any of the scalar fields in the Color by drop-down lists.

.

.

If you selected EnSight under Type, you will need to specify the EnSight Encas File Name. Use

Browse... to select the .encas file that was created when you exported the file with the File/Export...

ribbon tab option. If you do not make a selection, then you will need to create an appropriate .encas

file manually.

You can also select the number of Time Steps For EnSight Export. This number directly de-

termines how many time levels will be available for animation in EnSight.

.

Click Write... to open The Select File Dialog Box (p. ), in which you can specify a name and save a

file containing the pathline data.

To initiate saving pathline data through the text command interface enter the following TUI command:

display/path-lines/write-to-files

In addition to pathline data, you can also export particle data in either Standard, EnSight or Geo-

metry type. For information on exporting particle data in FIELDVIEW (standard), EnSight or .ibl

(geometry) format, refer to Exporting Steady-State Particle History Data (p. ).

...... Standard Type

If Standard is selected under Type, ANSYS Fluent will write the file in FIELDVIEW format, which can

be exported and read into FIELDVIEW. The FIELDVIEW ASCII Particle Path Format is licensed from

Intelligent Light, proprietor of an independent visualization software package (http://www.ilight.com).

The file name that you use for saving the data must have a .fvp extension. You also have the

ability to retrieve and display the particle and pathline trajectories from the file.

If the case is steady-state, the particle path information will be written in ASCII format. For transient

or unsteady-state cases, the BINARY format must be used. The FIELDVIEW file contains a set of

paths, where each path consists of a series of points. At every point the spatial location and selected

variables are defined. A full description of the ASCII and BINARY formats can be found in Appendix

K - Particle Path Formats of FIELDVIEW’s Reference Manual [] (p. ), available to licensed FIELDVIEW

users.

The following is an example of the FIELDVIEW format for a steady-state case:

FVPARTICLES

Tag Names

Variable Names

time

particle_id

. . . .

. . . .

. . . .

The beginning of the file displays header information. Tag Names cannot be specified when the

file is exported from ANSYS Fluent, and hence will always be . ANSYS Fluent enables you to export

two variables, which are listed under Variable Names: the first is determined by the scalar fields

selected in the Color by drop-down lists (time in the example above); the second is always

particle_id.

The rest of the file contains information about each path. A path section begins by listing the total

number of points for the path. Then a line of data is presented for each point, with the X, Y, and Z

locations listed in the first three columns and the variable information in the fourth and fifth columns.

The example above presents a single pathline consisting of three points; the time ranges from .

to ., and the ID of the particle is .

...... Geometry Type

If Geometry is selected under Type, the file will be written in .ibl format. The resulting file contains

particle paths in the form of a curve that can be read in GAMBIT. The following is an example of a

Geometry file format that contains multiple curves:

Closed Index Arclength

Begin section !

Begin curve !

. .

. -.

. -.

. -.

. -.

. -.

. -.

. -.

. -.

. -.

. -.

. -.

. -.

. .

The above example demonstrates how multiple curves can be imported; single curves may also be

imported. After importing this file into GAMBIT, the file is read by first looking for a Begin curve

string and then looking for the X, Y, and Z coordinates under the Begin curve line.

...... EnSight Type

By selecting EnSight under Type, you can generate files with the following extensions:

.mpg

.mscl

.encas

An .mpg file will be written for every time step specified in the Time Steps For EnSight Export

field. A sequential number will be appended to the .mpg extension to indicate the time step. Each

file contains a header that lists the time at which the data was exported, as well as three columns

listing the X, Y, and Z coordinates for every particle at that particular time step.

The following is an example of a file called particle.mpg0003, which contains data for nine

particles at the third time step:

File is written from fluent in ensight measured particle format for

t = .42813e-

particle coordinates

.27734e- .91710e- .69093e-

.75772e- .97040e- .92842e-

.26051e- .10134e- .63228e-

.16390e- .32442e- .23423e-

.32735e- .53326e- .70791e-

.69431e- .37006e- .27602e-

.77868e- .92054e- .11570e-

.78029e- .75717e- .13314e-

.54859e- .73727e- .23796e-

An .mscl file will be written for every time step specified in the Time Steps For EnSight Export

field. A sequential number will be appended to the .mscl extension to indicate the time step. Each

file contains the scalar information (specified under Color By) for every particle at a particular time

step.

The following is an example of a file called particle.mscl0006, which captures Particle ID data

for nine particles at the sixth time step:

particle id

.00000e+ .00000e+ .20000e+ .80000e+ .40000e+ .00000e+

.60000e+ .20000e+ .80000e+

A new .encas file will be written if a selection is made under EnSight Encas File Name. This new

file is a modified version of the .encas file selected with the Browse... button, and contains inform-

ation about all of the related files (including geometry, velocity, scalar and coordinate files). The

name of the new file will be the root of the original file with .new appended to it (for example if

test.encas is selected, a file named test.new.encas will be written). It is this new file that

should be read into EnSight.

The following is an example of a file called spray2-unsteady.new.encas, that refers to the

files generated when the data was originally exported as an EnSight Case Gold file type (.geo,

.vel, .sc11, and .sc12) and the files created during the pathline data export (.mpg and .mscl):

FORMAT

type: ensight gold

GEOMETRY

model: spray2-unsteady.geo

measured:  particle.mpg****

VARIABLE

scalar per measured node:  particle-id particle.mscl****

scalar per node: pressure                     spray2-unsteady.scl1

scalar per node: pressure-coefficient         spray2-unsteady.scl2

vector per node: velocity                     spray2-unsteady.vel

TIME

time set:  Model

number of steps:

filename start number:

filename increment:

time values: .00000e+ .21406e- .42813e- .64219e- .85626e-

.07032e- .28438e- .49845e- .71251e- .09266e-

In ANSYS Fluent you can determine the scalar field value at a particle location using the computed

cell-center values or values that have been interpolated to the nodes. By default, the Node Values

option is turned on, and the interpolated values are used. If you prefer to use the cell values, turn

the Node Values option off. Note that for face-only functions like Wall Shear Stress, the cell value

is the area-weighted average from the face values that define that cell as c0.

If you are plotting pathlines to show the effect of a porous medium or 2D fan boundary, to depict

.... Creating and Using Pathline Definitions

You can create named pathline definitions and save them for later use. See Creating and Using Contour

The steps for creating and using pathline definitions are similar to the Steps for Generating Path-

lines (p. ), with the addition of a field for naming the pathline definition.

Pathline definitions can be included in scenes as long as the XY Plot option is not enabled.

Note

You can move the colormap of a pathline definition by left-clicking and dragging it to the

desired location. The colormap can also be resized by dragging the corners of the box that

appears when you hover over the colormap. The colormap location is not saved with the

pathline definition.

Scenes can be used to display multiple graphics plots within a single window. For example, you could

overlay contours of pressure across a valve with velocity vectors and the mesh at the same location.

Scenes allow you to modify the transparency of each plot so that you can emphasize a particular plot

or view.

.... Generating a Scene

You can plot a scene made up of multiple graphics objects using the Figure . : The Scene Dialog

Box (p. ).

Results → Scene

New...

Figure . : The Scene Dialog Box

The basic steps for creating a scene:

Box (p. ).

New...

. (Optional) Enter a Name for the scene.

. (Optional) Enter a Title for the scene, which will appear in the graphics window tab where the scene is

displayed.

. Select the Graphics Objects that you want to include in the scene. If you want to include additional mesh,

contour, vector, or pathline plots in the scene, create them from the New Object drop-down list.

Note that pathlines with the XY Plot option enabled are not compatible with scenes.

. (Optional) You can modify the transparency of the selected graphics objects using the Transparency

slider. If the slider is completely to the right the object will be fully transparent.

. Click Save or Save & Display.

Scene Colormaps

Once the scene is displayed, you can move the colormaps by left-click and drag. Colormaps can also

be resized by dragging the corners of the box that appears when you hover over the colormap.

Tip

You can specify a different colormap scale for each graphic object to make it easier to

determine the values that correspond to the displayed gradients (to do this, click Colormap

Options... in the corresponding graphics object dialog box).

Sweep surfaces can be used when you want to examine the mesh, contours, or vectors on various

sections of the domain without explicitly creating the corresponding surfaces. For example, if you want

to display solution results for a 3D combustion chamber, instead of creating numerous surfaces at

different cross-sections of the domain, you can use a sweep surface to view the variation of the flow

and temperature throughout the chamber.

.... Steps for Generating a Plot Using a Sweep Surface

You can plot meshes, contours, or vectors on a sweep surface using the Sweep Surface Dialog

Box (p. ) (Figure . : The Sweep Surface Dialog Box (p. )).

Results → Animations → Sweep Surface

Edit...

Figure . : The Sweep Surface Dialog Box

The basic steps for generating a mesh, contour, or vector plot using a sweep surface are as follows:

.

Under Sweep Axis, specify the (X, Y, Z) vector representing the axis along which the surface should be

swept.

.

Click Compute to update the Min Value and Max Value to reflect the extents of the domain along the

specified axis.

.

Under Display Type, specify the type of display you want to see: Mesh, Contours, or Vectors.The first

time that you select Contours or Vectors, ANSYS Fluent will open the Contours Dialog Box (p. ) or

the Vectors Dialog Box (p. ) so you can modify the settings for the display.To make subsequent

modifications to the display settings, click Properties to open the Contours Dialog Box (p. ) or Vectors

.

Move the slider under Value (which indicates the value of x, y, or z) to move the sweep surface through

the domain along the specified Sweep Axis. ANSYS Fluent will update the mesh, contour, or vector

display when you release the slider.You can also enter a position in the Value field and press Enter to

update the display.

.

If you want to save the currently displayed sweep surface so that you can use it for a different type of

plot (for example, a pathlines plot or an XY plot) or combine it with displays on other surfaces, click

Create... to open the Create Surface Dialog Box (p. ) (Figure . :The Create Surface Dialog

Box (p. )). Enter the Surface Name and click OK.

Figure . : The Create Surface Dialog Box

The surface that is created is an isosurface based on the mesh coordinates; the contour or vector

settings are not stored in the surface.

You can also animate the sweep surface display, as described below, rather than moving the slide

bar yourself.

.... Animating a Sweep Surface Display

The steps for animating a sweep surface display are as follows:

.

Specify the Sweep Axis and Display Type as described above.

.

Under Animation, enter the Initial Value and Final Value for the animation.These values correspond

to the minimum and maximum values along the Sweep Axis for which you want to animate the display.

.

Specify the number of Frames you want to see in the animation.

.

Click Animate.

There may be situations where displaying graphics on a local machine is not practical. Therefore, you

may decide to hide (or disable) the graphics display window.

To disable the graphics display window when starting ANSYS Fluent from the command line, you can

specify the driver as null:

fluent -driver null

For an ANSYS Fluent session that is already in progress, the graphics window display can be disabled

using the following text command:

display → set → rendering-options → driver → null

Important

All graphics windows must be closed prior to invoking the previous text command.

If the graphics window display is disabled, you can continue to save graphics using the Save Picture

Important

option, as described in Saving Picture Files (p. ). Note that the speed at which the graphics are saved

may be significantly slower with the driver set to null, and the saved graphics files may not be

identical to those saved when the graphics window display is enabled.

For an ANSYS Fluent session that is already in progress, perform the following steps to re-enable a

graphics window display that had been previously disabled:

.

Enter the following text command:

display → set → rendering-options → driver

.

Press the Enter key at the driver> prompt to display the available drivers.

.

Enter an appropriate driver, such as opengl.

If any graphics windows are open (which are not visible to you), ANSYS Fluent will prompt you to close

all open windows. You can close them using the following Scheme command:

(close-all-open-windows)

and then retype the text command to enable the graphics windows.

Important

If you happen to be logged on to a machine remotely, then some drivers may not work on

your system. Use x11 (for Linux) or msw (for Windows) instead to enable your graphics

windows.

There are a number of ways in which you can alter the graphical display once you have generated the

basic elements in it (contours, meshes, and so on). For example, you can overlay multiple graphics, add

descriptive text or lighting to the plot, and modify the captions or legend layout. These and other cus-

tomizations are described in this section.

... Advanced Graphics Overlays

... Opening Multiple Graphics Windows

... Changing the Legend Display

... Adding Text to the Graphics Window

... Changing the Colormap

... Adding Lights

... Modifying the Rendering Options

Important

Normally, you can see only one picture at a time in the graphics window, unless you are Displaying a

Scene (p. ). Sometimes, however, you may want to create an "exploded" view, where results translated

or rotated out for the physical domain for enhanced display (see Figure . : Exploded Scene Display

of Temperature and Velocity (p. )). You can do this by turning on the Overlays option (and clicking

Apply) and using the transform operation in the Scene Description Dialog Box (p. ).

View → Graphics → Compose...

Once overlaying is enabled, subsequent graphics that you generate will be displayed on top of the

existing display in the active graphics window. To generate a plot without overlays, you must turn off

the Overlays option in the Scene Description Dialog Box (p. ) (and remember to click Apply).

When you are overlaying multiple graphics, the captions and color scale that will appear in the latest

display are those that correspond to the most recently drawn graphic.

Note that when overlaying is enabled, it will apply to all graphics windows, including those that are

not yet open. Turning overlays on and off does so for all graphics windows, not just for the active

window. That is, if you enable overlays, open a new graphics window (as described in Opening Multiple

Graphics Windows (p. )), and then generate two or more graphics in that window, they will be

overlaid.

Customizing the Graphics Display

Figure . : Exploded Scene Display of Temperature and Velocity

During your ANSYS Fluent session, you can open up to  graphics windows at one time and they

may be viewed within the application window or in separate windows. The windows are numbered

through  and the ID number for each window will appear at the top of the frame that surrounds it.

You can view a specific window by selecting it from the drop-down list next to the ID number. The

first time you display graphics, window  will be displayed automatically. To open an additional window,

you can use the Display Options Dialog Box (p. ) (Figure . : The Display Options Dialog Box (p. )).

Results → Graphics

Options...

Figure . : The Display Options Dialog Box

Use the up arrow to increment the window ID in the Active Window field under Graphics Window

and then click Open. The Close button changes to the Open button if the Active Window is set to

more than .

To close an open window, increase or decrease the Active Window value to the ID of the window to

be closed, and then click Close that appears next to the Active Window field. The Open button

changes to a Close button if the Active Window is open.

.... Setting the Active Window

When you have more than one graphics window open, you must identify the active window so that

ANSYS Fluent will know which one to draw the plot in. There are two ways to set the active window:

you can simply click any mouse button in the desired graphics window, or you can specify the ID for

the desired graphics window in the Active Window field (in the Display Options Dialog Box (p. ))

and click Set. Regardless of the method used, this window will remain active until you set a new

active window.

ANSYS Fluent graphics include, by default, a caption or legend block that consists of fields of text de-

scribing the contents of the graphic, the ANSYS Fluent product identification, an axis triad indicating

the orientation of the displayed object, a color key defining the correspondence between each color

and the magnitude of the plotted variable, and the ANSYS logo. You can turn off the display of the

legend and color scale, and/or the axis triad. You can also hide the ANSYS logo. You can also display

the colormap on any side of the display window as per convenience. In addition you can also edit the

captions directly in the graphics window.

.... Controlling the Titles, Axes, Ruler, Logo, and Colormap

You can enable/disable the display of the Titles, Axes, and Ruler directly in the graphics window by

toggling the appropriate icon (refer to Additional Display Options (p. ) for more information). The

Logo and the Colormap are controlled under Layout in the Display Options Dialog Box (p. ) (Fig-

ure . : The Display Options Dialog Box (p. )).

Use the text interface to enable/disable the captions and color scale individually, and to change the

size and position of the captions and color scale.

display → set → windows → text →

display → set → windows → scale →

See the separate Text Command List for details.

Controlling Titles

You can add text, such as your company name, to the title box in multiple locations using the dis-

play/set/titles/ text command locations. Once you have provided text for one of these locations,

you must ensure that display/set/windows/text/company? is set to yes, then re-render the

display by displaying a graphics object (for example, mesh, contour, vector, and so on) or by entering

display/re-render in the console.

Alternatively, if you always want your company name or other text displayed in the title box, you can

set the FLUENT_COMPANY environment variable in the Fluent Launcher equal to your company

name or the desired text, for example, FLUENT_COMPANY=My Example Company Name. Note

that Titles is disabled by default when you launch Fluent, so you will have to enable Titles before it will

be displayed in the graphics window.

.... Editing the Legend

When captions are displayed in the graphics window, you may choose to modify, delete, or add to

the text that appears in the caption box. To do so, click the left mouse button in the desired location.

A cursor will appear, and you can then type new text or delete the text that was originally there (using

the backspace or delete key). Note that changes to existing text in the caption block will be removed

when you draw new graphics in the window (unless you are overlaying multiple graphics in the same

window), but text that you add on a previously empty line in the caption block will not be removed

until the default caption text makes use of that line.

.... Adding a Title to the Caption

You can define a title for your problem using the title text command:

display → set → title

The title you define will appear on the top line of the caption, at the far left, in all subsequent plots.

It will also be saved in the case file.

Important

You will need to enclose your title in quotation marks (for example, " my title ").

.... Enabling/Disabling the Axes

You can disable the display of the axis triad by turning off the Axes Visibility button (

) in the

.... Enabling/Disabling the Ruler

You can disable the display of the ruler by turning off the Ruler Visibility button (

) in the

Note that if your project is 3D, then enabling the ruler automatically changes the view to orthographic

so that the ruler markings are relevant for the model.

.... Modifying and Displaying/Hiding the Logo

The graphics window displays a white ANSYS logo in the upper right corner. You may choose between

a white (default) or black logo by selecting White or Black from the Color drop-down list under

Layout in the Display Options Dialog Box (p. ) (Figure . : The Display Options Dialog Box (p. )).

You can prevent the ANSYS logo from being displayed in the graphics window by disabling the Logo

option under Layout.

.... Colormap Alignment

You can set the position of the colormap on any side (left, top, bottom, or right) of the display window.

Default alignment for the colormap is set to the Left. If you want to change the alignment, select the

required direction in the Colormap Alignment drop-down list.

You can use the Annotate Dialog Box (p. ) to add text to the graphics window with optional attach-

ment lines. Figure . : Graphics Window with Text Annotation (p. ) shows an example of a

graphics display with annotated text in it.

Figure . : Graphics Window with Text Annotation

.... Adding Text Using the Annotate Dialog Box

Adding text to the graphics window using the Annotate Dialog Box (p. ) (Figure . : The Annotate

Dialog Box (p. )) enables you to control the font and color of the text.

Annotate...

Figure . : The Annotate Dialog Box

The steps for adding text are as follows:

.

Under Font Specification, select the font type in the Name drop-down list, the font weight (Medium

or Bold) in the Weight drop-down list, the size (in points) in the Size drop-down list, the color in the

Color drop-down list, and the slant (Regular or Italic) in the Slant drop-down list.

.

.

Enter the text that you want to add in the Annotation Text field.

.

Click Add.You will be asked to pick the location in the graphics window where you want to place the

text, using the mouse-probe button. By default, the mouse-probe button is the right button, but you

can change this in the Mouse group box of the View tab, as described in Controlling the Mouse Button

If you click the mouse button once in the desired location, the text will be placed at that point.

Dragging the mouse with the mouse-probe button depressed will draw an attachment line from

the point where the mouse was first clicked to the point where it was released. The annotation

text will be placed at the point where the mouse button was released.

.... Editing Existing Annotation Text

Once you have added text to the graphics display, you may change the font characteristics of one

or more text items, or delete individual text items.

To modify or delete existing text, follow these steps:

.

Select the appropriate item in the Names list in the Annotate Dialog Box (p. ) (Figure . :The An-

notate Dialog Box (p. )).When you select a name, the associated text will be displayed in the Annota-

tion Text field, and the Add button becomes the Edit button.

.

Modify the Font Specification entries as desired, and click Edit to modify the text, or simply click Delete

Text below the Names list to delete the selected text.

Note that if you want to make changes to all current annotation text, you can select all of the Names

instead of just one in step .

You can move the text in the same way that you move other geometric objects in the display, using

the Scene Description Dialog Box (p. ) and the Transformations Dialog Box (p. ). See Transforming

Geometric Objects in a Scene (p. ) for details.

.... Clearing Annotation Text

Annotation text is associated with the active graphics window and is removed only when the annota-

tions are explicitly cleared. To remove the annotations from the graphics window, you must click

Clear in the Annotate Dialog Box (p. ). If you draw new graphics in the window without clearing

the annotations, they will remain visible in the new display.

The default colormap used by ANSYS Fluent to display graphical data (for example, vectors) ranges

from blue (minimum value) to red (maximum value). Additional predefined colormaps are available,

and you can also create custom colormaps. To make any changes to the colormap, you will use the

Colormap Dialog Box (p. ) (Figure . : The Colormap Dialog Box (p. )).

Colormap...

Figure . : The Colormap Dialog Box

When you plot contours, you can temporarily modify the number of colors in the colormap by changing

the number of contour levels in the Contours Dialog Box (p. ); you will only need to use the Colormap

Dialog Box (p. ) if you want to change other characteristics of the colormap.

Important

Note that if you are using a gray-scale colormap and you want to save a gray-scale picture,

you should save a color picture. When you save a gray-scale picture, ANSYS Fluent uses an

Important

internal gray scale, not the gray scale specified by the colormap. If you save a color picture,

the colormap you selected (that is, your gray scale) will be used.

.... Predefined Colormaps

The following colormaps are automatically available in ANSYS Fluent:

bgr:

Blue represents the minimum value, green the middle, and red the maximum value. Colors in between

are interpolated from blue to green, and from green to red. (This is the default colormap.)

bgrb:

Blue represents the minimum and maximum values, and green and red are values / and / of the

maximum value, respectively. Colors in between are interpolated from blue to green, from green to red,

and from red to blue.

blue:

The minimum value is represented by blue-black, and the maximum value by pure blue.

cyan-yellow:

Cyan represents the minimum value and yellow represents the maximum value.

fea:

Blue represents the minimum value and red represents the maximum value.The colors in between are

those used in third-party finite element analysis packages.

gray:

Black is used for the minimum value and white for the maximum value.

green:

The minimum value is represented by green-black, and the maximum value by pure green.

purple-magenta:

Purple represents the minimum value and magenta represents the maximum value.

red:

The minimum value is represented by red-black, and the maximum value by pure red.

rgb:

Red represents the minimum value, green the middle, and blue the maximum value. Colors in between

are interpolated from red to green, and from green to blue.

rgb:

The number of colors interpolated between the colors in the scale name (for example, between purple

and magenta) will depend on the size of the colormap.

.... Selecting a Colormap

The procedure for selecting a new colormap to be used in graphics displays is as follows:

.

In the Colormap Dialog Box (p. ) (Figure . :The Colormap Dialog Box (p. )), select the desired

colormap in the Currently Defined drop-down list.This list will contain all of the colormaps predefined

by ANSYS Fluent as well as any custom colormaps that you have created as described in Creating a

Customized Colormap (p. ).

.

Set the colormap size and scale as described in Specifying the Colormap Size and Scale (p. ).

.

Click Apply to update the current graphics display with the new colormap. All future displays will use

the newly selected colormap and options.

..... Specifying the Colormap Size and Scale

Once you have selected the desired colormap from the Currently Defined list, you may modify the

Colormap Size. This value is the number of distinct colors in the color scale.

You can also choose to use a logarithmic scale instead of a decimal scale by turning on the Log

Scale option. With a log scale, the color used in the graphics display will represent the log of the

value at that location in the domain. The values represented by the colors will, therefore, increase

exponentially.

..... Changing the Number Format

You can change the format of the labels that define the color divisions at the left of the graphics

window using the controls under the Number Format heading in the Colormap Dialog Box (p. ).

To display the real value with an integral and fractional part (for example, . ), select float in the

Type drop-down list.You can set the number of digits in the fractional part by changing the value of

Precision.

To display the real value with a mantissa and exponent (for example, .0e-), select exponential in the

Type drop-down list.You can define the number of digits in the fractional part of the mantissa in the

Precision field.

To display the real value with either float or exponential form, depending on the size of the number and

the defined Precision, choose general in the Type drop-down list.

.... Displaying Colormap Label

You can customize the number of values displayed on the colormap. The default number of labels

that appear alongside the colormap depends on the font size and the colormap size (Figure . : The

Default Colormap Label Display (p. )).

To reduce the number of labels that appear alongside the colormap, increase the number of labels

skipped.To do so, deselect Show All in the Colormap Dialog Box (p. ) and set the number of labels

to be skipped.

To demonstrate what effect this command has on the display, enter a value of  under Skip

(note that the value entered must be an integer). This will result in three intermediate labels

being skipped, with the first and the last colormap values always being displayed (Fig-

ure . : The Colormap with Skipped Labels (p. )).

To reset the original colormap display, simply select Show All.

Figure . : The Default Colormap Label Display

Figure . : The Colormap with Skipped Labels

.... Creating a Customized Colormap

You can create your own colormap by manipulating the “anchor colors” and the colormap size. A

color scale is created by linear interpolation between the anchor colors. The color, number, and pos-

ition of the anchor colors will therefore control the description of the colormap. By increasing the

colormap size, you can increase the total number of colors and obtain a color scale that changes

more gradually. The procedure is as follows:

.

In the Colormap Dialog Box (p. ), click Edit... to open the Colormap Editor Dialog Box (p. ) (Fig-

ure . :The Colormap Editor Dialog Box (p. )).

Figure . : The Colormap Editor Dialog Box

.

In the Colormap Editor Dialog Box (p. ), select a color scale in the Currently Defined list as your

starting point.The colors in the scale will be displayed at the top of the dialog box. A white bar below

a color is an "anchor point" indicating that this color is an "anchor color".

.

If you want to add more colors to the color scale, increase the Colormap Size; to use fewer colors, de-

crease this value.When you use the counter arrows (or type in a value and press Enter), the color scale

display at the top of the dialog box will be updated immediately.

Important

The total number of colors must not be less than the number of anchor points.

.

To obtain the desired color scale interpolation, manipulate the anchor colors as needed:

To add an anchor point, click any mouse button on the black space directly below the desired anchor

.

color (or click the color itself). A white bar will appear below the color to identify it as an anchor color,

and the color will automatically be selected for color-definition modification.

To remove an anchor point, click the white bar below the anchor color.The white bar will disappear

and the color scale will be updated to reflect the new interpolation.

To select a current anchor color in order to modify its color definition, click the color itself at the top

of the dialog box.

To modify the color of the selected anchor color, you can change either the red/green/blue compon-

ents (choose RGB, the default) or the hue/saturation/value components (choose HSV). HSV is recom-

mended if you plan to record the graphics display on video, as it enables you to create a more subtle

gradation of color and reduce the tendency of bright colors to “bleed”. Move the Red, Green, and

Blue or Hue, Saturation, and Value sliders to obtain the desired color.The color scale at the top of

the dialog box will be updated automatically to show the effect of your change.

Important

It is a good idea to note the original value of a color component before moving

the slider so that you will be able to return to it if you change your mind. (See

Scales (p. ) for instructions on using a scale slider.)

If you make a mistake while modifying the color scale, you can start over by selecting the starting-

point colormap in the Currently Defined list.

.

If you want to change the default name of the new colormap, enter the new name in the Name field.

.

By default, custom colormaps are called cmap-, cmap-, and so on.

.

Click OK to save the new colormap.The colormap name appears in the Currently Defined list in the

Colormap Dialog Box (p. ) and can be selected for use in the graphics display.

Custom colormap definitions will be saved in the case file.

In ANSYS Fluent you can add lights with a specified color and direction to your display. These lights

can enhance the appearance of the display when it contains 3D geometries. By default one light is

defined. You can enable the effect of the existing light(s) using the Display Options Dialog Box (p. )

or the Lights Dialog Box (p. ), and you can add new lights using the Lights Dialog Box (p. ).

....Turning on Lighting Effects with the Display Options Dialog Box

To enable the effect of lighting, you can use the Display Options Dialog Box (p. ).

If you enable the Lights On option under Lighting Attributes and click Apply, you will see the

lighting effects in the active graphics window. To turn off the lighting effects, simply turn off the

Lights On option and click Apply.

You can also choose the method to be used in lighting interpolation; select Flat, Gouraud, or Phong

in the Lighting drop-down list. Flat is the most basic method: there is no interpolation within the

individual polygonal facets. Gouraud and Phong have smoother gradations of color because they in-

terpolate on each facet.

....Turning on Lighting Effects with the Lights Dialog Box

You can also enable lighting effects using the Lights Dialog Box (p. ) (Figure . : The Lights Dialog

Box (p. )).

Box (p. )).

Lights...

For constant lighting effects in the direction of the view, enable the Headlight On option in the

Lights Dialog Box (p. ). This option has the effect of a light source directly in front of the model,

no matter what orientation the model is viewed in. To disable this feature, turn off the Headlight

On option in the Lights Dialog Box (p. ).

In the Lighting Method drop-down list, choose Flat, Gouraud, or Phong to enable the appropriate

lighting method. These methods are described in the previous section. To disable lighting, select Off

in the list. To see the lighting effects in the active graphics window, click Apply.

.... Defining Light Sources

You can control individual lights in the Lights Dialog Box (p. ) (Figure . : The Lights Dialog

Box (p. )). The Lights Dialog Box (p. ) enables you to create a light and then turn it off without

deleting it. In this way, you can retain lights that you have defined previously but do not want to use

at present.

Lights...

Figure . : The Lights Dialog Box

(You can also open the Lights Dialog Box (p. ) by clicking Lights... in the Display Options Dialog

Box (p. ).)

By default, light  is defined to be dark gray with a direction of (,,). A light source is a distant light,

similar to the sun. The direction (,,) means that the rays from the light will be parallel to the vector

from (,,) to the origin. To create an additional light (for example, light ), follow the steps listed

below.

.

.

below.

.

.

Enable the Light On check box.

.

.

Enter the (X, Y, Z) Cartesian components under Direction.

Click the middle mouse button in the desired location on the sphere under Active Lights. (You can

also move the light along the circles on the surface of the sphere by dragging the mouse while

holding down the middle button.) You can rotate the sphere by pressing the left mouse button and

moving the mouse (like a trackball).

Use your mouse to change the view in the graphics window so that your position in reference to the

geometry is the position from which you would like a light to shine.Then click Use View Vector to

update the X,Y,Z fields with the appropriate values for your current position and update the graphics

display with the new light direction.This method is convenient if you know where you want a light

to be, but you are not sure of the exact direction vector.

.

.

When you have defined all the lights you want, click Apply to save their definitions.

..... Removing a Light

clear the Light On check box. When a light is turned off, its definition is retained, so you can easily

add it to the display again at a later time by selecting the Light On check box. For example, you

may want to define three different lights to be used in different scenes. You can define each of

them, and then enable only one or two at a time, using the Light ID field and the Light On check

box. Once you have made all the desired modifications to the lights, remember to click Apply to

save the changes.

..... Resetting the Light Definitions

If you have made changes to the light definitions, but you have not yet clicked Apply, you can reset

the lights by clicking Reset. All lighting characteristics will revert to the last saved state (that is, the

lighting that was in effect the last time you opened the dialog box or clicked on Apply).

Depending on the objects in your display window and what kind of graphics hardware and software

you are using, you may want to modify some of the rendering parameters listed below. All are listed

under the Rendering heading in the Display Options Dialog Box (p. ) (Figure . : The Display

After making a change to any of these rendering parameters, click Apply to re-render the scene in

the active graphics window with the new attributes. To see the effect of the new attributes on another

graphics window, you must redisplay it or make it the active window (see Setting the Active Win-

dow (p. )) and click Apply again.

Line Width:

By default, all lines drawn in the display have a thickness of  pixel. If you want to increase the thickness

of the lines, increase the value of Line Width.

Point Symbol:

By default, nodes displayed on surfaces and data points on line or rake surfaces are represented in the

display by a + sign inside a circle. If you want to modify this representation (for example, to make the

nodes easier to see), you can select a different symbol in the Point Symbol drop-down list.

Animation Options:

There are two animation options that you can choose from.They are as follows:

All

Wireframe

Double Buffering:

Outer Face Culling:

Hidden Surface Removal:

If you do not use hidden surface removal, ANSYS Fluent will not try to determine which surfaces in the

display are behind others; it will display all of them, and a cluttered display will result for most 3D mesh

displays. For most 3D problems, therefore, you should enable the Hidden Surface Removal option.You

should turn this option off (for optimal performance) if you are working with a 2D problem or with geo-

metries that do not overlap.

is the fastest method if your hardware supports it.The accuracy and speed of this method is hardware-

dependent. Note that if this method is not available on your computer, selecting it will cause the

Software Z-buffer method to be used.

Painters

will show fewer edge-aliasing effects than Hardware-Z-buffer.This method is often used instead of

Software-Z-buffer when memory is limited.

memory-intensive.

is a fast software method, but it is not as accurate as Software-Z-buffer.

.... Graphics Device Information

you can click Info in the Display Options Dialog Box (p. ). The graphics device information will be

printed in the text (console) window.

A convenient feature of ANSYS Fluent is that it enables you to assign a specific function to each of the

mouse buttons. According to your specifications, clicking a mouse button in the graphics window will

cause the appropriate action to be taken. These functions apply only to the graphics windows; they

behave differently when an XY plot or histogram is displayed. For information about the use of mouse

buttons in these plots, see Plot Types (p. ). Clicking any mouse button in a graphics window will

make that window the active window.

Important

3Dconnexion Space products (Mouse, Pilot, and Navigator) are not supported with ANSYS

Fluent.

... Button Functions

... Modifying the Mouse Button Functions

The predefined button functions available are listed below:

Enables you to rotate the view by dragging the mouse across the screen. Dragging horizontally rotates

the object about the screen’s -axis; vertical mouse movement rotates the object about the screen’s

axis.The function completes when the mouse button is released or the cursor leaves the graphics

window.

Enables you to translate the view by dragging the mouse while holding down the button.The function

Controlling the Mouse Button Functions

mouse-scroll-zoom (non-modifiable)

Enables you to use the middle scroll-wheel to zoom in and out on the graphics window based on the

location of the mouse pointer.

Enables you to draw a zoom box, anchored at the point at which the button was pressed, by dragging

the mouse with the button held down.When you release the button, if the dragging was from left to

right, a magnified view of the area within the zoom box will fill the window. If the dragging was from

right to left, the area of the window is shrunk to fit into the zoom box, resulting in a “zoomed out” view.

If the mouse button is simply clicked (not dragged), the selected point becomes the center of the window.

Enables you to rotate or zoom the view, depending on the direction in which you drag the mouse. If you

drag the mouse horizontally, the display will rotate about the axis normal to the screen. If you drag it

vertically, the display will be magnified (if you drag it down) or shrunk (if you drag it up).The function

Enables you to select items from the graphics windows and request information about displayed scenes.

If you have selected short description from the Probe drop-down list and then click the mouse-probe

button in the graphics window, only the identity of the item on which you clicked will be printed out in

the console; if you have selected long description instead, more detailed information about a selected

item will be displayed.

Note

A left-click will always select unless the left-mouse-button is set as mouse-zoom or mouse-

Note

probe.

Mouse button functions are specified in the View tab.

View

For each mouse button (Left, Middle, and Right), select the desired function in the drop-down list.

The functions are listed above. If you assign the probe function to one of the buttons, select short

description or long description from the Probe drop-down list to indicate the amount of detail you

want displayed in the console.

The new button functions take effect as soon as they are changed. That is, you do not have to redraw

the graphics window to use the new functions; the appropriate function will be executed when a

mouse button is subsequently clicked in a graphics window.

The ANSYS Fluent Defaults button functions are as follows:

3D Action

2D Action

Operation

Key

Mouse Button

Rotate

Pan/dolly

Drag

Left

Select

Select

Click

Left

Add or remove selection

Click

Ctrl

Left

Zoom

Zoom

Scroll

Middle

Box-zoom

Box-zoom

Drag

Middle

Box-zoom

Box-zoom

Drag

Shift

Middle

Pan/dolly

Pan/dolly

Drag

Ctrl

Middle

Probe/context menu

Click

Right

Drag

Right

Click

Shift

Right

The Workbench Defaults button functions are as follows:

3D Action

2D Action

Operation

Key

Pan/dolly

Pan/dolly

Drag

Left

Select

Select

Click

Left

Click

Ctrl

Left

Zoom

Zoom

Scroll

Middle

Rotate

Probe

Drag

Middle

Box-zoom

Probe

Drag

Shift

Middle

Pan/dolly

Probe

Drag

Ctrl

Middle

Context menu

Click

Ctrl

Left

Zoom

Zoom

Scroll

Middle

Rotate

Probe

Drag

Middle

Box-zoom

Probe

Drag

Shift

Middle

Pan/dolly

Probe

Drag

Ctrl

Middle

Click

Right

Zoom

Zoom

Drag

Right

Fit to center

Click

Shift

Right

In ANSYS Fluent, the application window houses the ribbon and console, as well as multiple graphics

windows, task pages, and the tree. By default, all components are displayed and one graphics window

is visible. You can toggle the visibility of the toolbars, task page, console, and graphics window using

in the standard toolbar. The ribbon and the tree are never fully hidden—you can hide the ribbon

contents using

(also in the standard toolbar), but the tab names are always visible. You also have

the option of viewing separate graphics windows as described in Opening Multiple Graphics Win-

dows (p. ). For additional information about the various elements of the application window, see

Graphical User Interface (GUI) (p. ).

ANSYS Fluent enables you to select and control the view of the scene that is displayed in the graphics

window. You can modify the view by scaling, centering, rotating, translating, or zooming the display.

Modifying the View

You can also save a view that you have created, or restore or delete a view that you saved earlier. These

operations are performed in the Views Dialog Box (p. ) (Figure . : The Views Dialog Box (p. ))

or with the mouse, or simply using the shortcut in the graphics toolbar, as described in Selecting a

View (p. ).

Important

You can revert to the previous view by pressing Ctrl+L while the graphics window has the

View (p. ).

Important

main focus. You can also use the text command view last from the top level of the text

command tree. You can use the command to revert to any of the past  views.

... Selecting a View

... Manipulating the Display

... Saving and Restoring Views

... Mirroring and Periodic Repeats

You can use the Views Dialog Box (p. ) (Figure . : The Views Dialog Box (p. )) to select the

orientation of your display or use the

drop-down available in the graphics toolbar for 3D simula-

tions. Furthermore, you can simply click the interactive triad (Figure . : Using the Triad to Change

the Orientation of the Object (p. )), displayed in the graphics window. The Table . : Standard

Views (p. ) relates the Views listed in the Views Dialog Box (p. ) to the views available in the

graphics toolbar (see Pointer Tools (p. )).

Views...

Table . : Standard Views

View Shortcut in Graphics

Toolbar

View Listed in

Dialog Box

back

bottom

front

isometric

left

right

top

Figure . : Using the Triad to Change the Orientation of the Object

To change the orientation of the object in the graphics window using the triad (Figure . : Using

the Triad to Change the Orientation of the Object (p. )), you can

Click an axis/semi-sphere to point it in the positive/negative direction.

Right-click an axis/semi-sphere to point it in the negative/positive direction.

Click the white rotational arrows at the bottom of the triad to perform in-plane clockwise or counterclockwise

degree rotations.

Left-click and hold—in the vicinity of the triad—and use the mouse to perform free-rotations in any direction.

Release left mouse button to stop rotating.

Note that clicking on the X-axis will result in the +X-axis pointing towards you.

Note

For 2D cases, the

drop-down and the interactive triad are not available; in a front view,

the X-axis is horizontal with the positive direction to the right, the Y-axis is vertical with the

positive direction pointing up, and the Z-axis is determined by the right-hand rule.

Most of the manipulating activities (like scaling and centering the display) are accomplished using the

Views Dialog Box (p. ) (Figure . : The Views Dialog Box (p. )).

Views...

Figure . : The Views Dialog Box

You can rotate, translate, and zoom the graphics display using either the mouse or the Camera Para-

meters Dialog Box (p. ) (Figure . : The Camera Parameters Dialog Box (p. )), which is opened

from the Views Dialog Box (p. ).

Figure . : The Camera Parameters Dialog Box

.... Scaling and Centering

You can scale and center the current display without changing its orientation by clicking Auto Scale

in the Views Dialog Box (p. ).

.... Rotating the Display

Use either the mouse or the Camera Parameters Dialog Box (p. ) to:

Rotate the display in any direction (in 3D)

Rotate the display about the axis normal to the screen (in 2D)

To rotate a display with the mouse, use the button with the mouse-rotate function (the left button,

by default). For information about changing the mouse functions, see Controlling the Mouse Button

Click and drag the left mouse button in the graphics window to rotate the geometry in the display.

You can also click and drag the left mouse button on the ( ,

, ) graphics triad in the lower left

corner to rotate the display.

If you press the Shift key when you first click the mouse button to begin the rotation, the rotation

will be constrained to a single direction (for example, you can rotate about the screen’s horizontal

axis without changing the position relative to the vertical axis).

If you want to constrain the rotation of a display to be about the axis normal to the screen, you can

also use the mouse-roll-zoom function.

Click the appropriate mouse button and drag the mouse to the left for clockwise rotation, or to the

right for counterclockwise rotation.

To rotate a 3D display using the Camera Parameters Dialog Box (p. ) (Figure . : The Camera

Parameters Dialog Box (p. )) use the dial and the slider of the scales.

To rotate about the horizontal axis at the center of the screen, move the slider on the scale to the left of

the dial up or down (see Scales (p. ) or instructions on using the scale).

To rotate about the vertical axis at the center of the screen, move the slider on the scale below the dial

to the left or right.

To rotate about the axis at the center of and perpendicular to the screen, click the left mouse button on

the indicator in the dial and drag it around the dial.

Important

The position of the slider or the dial indicator does not reflect the cumulative rotation

about the axis as the slider/indicator will return to its original position when you release

the mouse button.

..... Spinning the Display with the Mouse

When you use the mouse for rotation, you have the option to “push” the display into a continuous

spin. This feature can be used in conjunction with video recording, or simply for interactive viewing

of the domain from different angles. To use this option, use the auto-spin? text command:

display → set → rendering-options → auto-spin?

Then display the graphics (or, if the graphics are already displayed, you can click Apply in the Display

Options Dialog Box (p. )). The mouse-rotate button will then have two uses:

To perform the standard rotation, stop dragging the mouse before you release the mouse-rotate button.

To start the continuous spin, release the mouse-rotate button while you are still dragging the mouse.

The display will continue to rotate on its own until you click any mouse button in the graphics window

again.The speed of the rotation will depend on how fast you are dragging the mouse when you release

the button.

For smoother rotation, enable the Double Buffering option in the Display Options Dialog Box (p. )

(see Modifying the Rendering Options (p. )). This will reduce screen flicker during graphics updates.

....Translating the Display

By default the left mouse button is set to mouse-dolly in 2D. For information about changing the

mouse functions, see Controlling the Mouse Button Functions (p. ). Click and drag the left mouse

button in the graphics window to translate the geometry in the display.

In 3D, you can either change one of the button functions to mouse-dolly and follow the instructions

above for 2D, or use the mouse-zoom button (the middle button by default). Click the middle button

once on the point in the display that you want to move to the center of the screen. ANSYS Fluent will

redisplay the graphic with that point in the center of the window. This method can also be used in

2D.

.... Zooming the Display

In both 2D and 3D you will use the mouse button with the mouse-zoom function (the middle button

by default) or the mouse-roll-zoom function (see Controlling the Mouse Button Functions (p. )

for information about enabling this optional function), or the Camera Parameters Dialog Box (p. )

to magnify and shrink the display.

With the mouse-zoom function, click the middle mouse button and drag it from left to right (creating

a "zoom box") to magnify the display. Figure . : Zooming In (Magnifying the Display) (p. ) displays

the correct dragging of the mouse, from upper left to lower right on the display, in order to zoom.

You can also drag from lower left to upper right. After you release the mouse button, ANSYS Fluent will

redisplay the graphic, filling the graphics window with the portion of the display that previously oc-

cupied the zoom box.

Figure . : Zooming In (Magnifying the Display)

Figure . : Zooming Out (Shrinking the Display)

Click the middle mouse button and drag it from right to left to shrink the display. Figure . : Zooming

Out (Shrinking the Display) (p. ) displays the correct dragging of the mouse, from lower right to

upper left on the display, in order to "zoom out". You can also drag from upper right to lower left.

After you release the mouse button, ANSYS Fluent will redisplay the graphic, shrinking the graphical

display by the ratio of sizes of the zoom box you created and the previous display.

With the mouse-roll-zoom function, click the appropriate mouse button and drag the mouse down

to zoom in continuously, or up to zoom out. In the Camera Parameters Dialog Box (p. ) (Fig-

ure . : The Camera Parameters Dialog Box (p. )), use the scale to the right of the dial to zoom

the display. Move the slider bar up to zoom in and down to zoom out.

Perspective and other camera parameters are defined in the Views Dialog Box (p. ), which you can

open by clicking Camera... in the Camera Parameters Dialog Box (p. ) (Figure . : The Views Dialog

Box (p. )).

Views...

.... Perspective and Orthographic Views

You may choose to display either an orthographic view or a perspective view of your graphics. To

show a perspective view (the default), select Perspective in the Projection drop-down list in the

Views Dialog Box (p. ) (Figure . : The Camera Parameters Dialog Box (p. )). To turn off per-

spective, select Orthographic in the Projection drop-down list.

.... Modifying Camera Parameters

Instead of translating, rotating, and zooming the display as described in Manipulating the Dis-

play (p. ), you may sometimes want to modify the “camera” through which you are viewing the

graphics display.

The camera is defined by four parameters: position, target, up vector, and field, as illustrated in Fig-

ure . : Camera Definition (p. ). "Position" is the camera’s location. "Target" is the location of the

point the camera is looking at, and "up vector" indicates to the camera which way is up. "Field" indicates

the field of view (width and height) of the display.

To modify the camera’s position, select Position in the Camera drop-down list and specify the X, Y,

and Z coordinates of the desired point. To modify the target location, select Target in the Camera

drop-down list and specify the coordinates of the desired point. Select Up Vector to change the up

direction. The up vector is the vector from (,,) to the specified (X,Y,Z) point. Finally, to change the

field of view, select Field in the Camera list and enter the X (horizontal) and Y (vertical) field distances.

Important

Click Apply after you change each camera parameter (Position, Target, Up Vector, and

Field).

After you make changes to the view shown in your graphics window, you may want to save the view

so that you can return to it later. Several default views are predefined for you, and can be easily restored.

All saving and restoring functions are performed with the Views Dialog Box (p. ) (Figure . : The

Views Dialog Box (p. )).

Views...

Important

Note that settings for mirroring and periodic repeats are not saved in a view.

.... Restoring the Default View

When experimenting with different view manipulation techniques, you may accidentally "lose" your

geometry in the display. You can easily return to the default (front) view by clicking Default in the

Views Dialog Box (p. ).

.... Returning to Previous Views

After manipulating the display and viewing it from different angles, you can return to previous displays

by clicking Previous in the Views Dialog Box (p. ).

.... Saving Views

Once you have created a new view that you want to save for future use, enter a name for it in the

Save Name field in the Views Dialog Box (p. ) and click Save. Your new view will be added to the

list of Views, and you can restore it later as described below.

If a view with the same name already exists, you will be asked in a Question Dialog Box (p. ) if it

is OK to overwrite the existing view. If you overwrite one of the default views (top, left, right, front,

and so on), be sure to save it in a view file if you want to use it in a later session. Although all views

are saved to the case file, the default views are recomputed automatically when a case file is read in.

Any custom view with the same name as a default view will be overwritten at that time.

As mentioned previously, all defined views will be saved in the case file when you write one. If you

plan to use your views with another case file, you can write a “view file” containing just the views.

You can read this view file into another Fluent session involving a different case file and restore any

of the defined views, as described below.

To save a view file, click Write... in the Views Dialog Box (p. ). In the resulting Write Views Dialog

Box (p. ) (Figure . : The Write Views Dialog Box (p. )), select the views you want to save in

the Views to Write list and click OK. You will then use the Select File dialog box to specify the file

name and save the view file. See The Select File Dialog Box (p. ) for more details.

Figure . : The Write Views Dialog Box

.... Reading View Files

If you have saved views to a view file (as described above), you can read them into your current Fluent

session by clicking Read... in the Views Dialog Box (p. ), and indicating the name of the view file

in The Select File Dialog Box (p. ). If a view that you read has the same name as a view that already

exists, you will be asked in a Question Dialog Box (p. ) if it is OK to overwrite (that is, replace) the

existing view.

.... Deleting Views

If you decide that you no longer want to keep a particular view, you can delete it by selecting it in

the Views list and clicking on Delete. Use this option carefully, so that you do not accidentally delete

one of the predefined views.

If you model the problem domain as a subset of the complete geometry using symmetry or periodic

boundaries, you can display results on the complete geometry by mirroring or repeating the domain.

For example, only one half of the annulus shown in Figure . : Mirroring Across a Symmetry

Boundary (p. ) was modeled, but the graphics are displayed on both halves. You can also define

mirror planes or periodic repeats just for graphical display, even if you did not model your problem

using symmetry or periodic boundaries.

Figure . : Mirroring Across a Symmetry Boundary

Display of symmetry and periodic repeats is controlled in the Views Dialog Box (p. ) (Figure . : The

Views...

For a symmetric domain, all symmetry boundaries are listed in the Mirror Planes list. Select one or

more of these boundaries as the plane(s) about which to mirror the display.

For a periodic domain, click Define... to open the Graphics Periodicity Dialog Box (p. ), to access

the periodicity parameters. Specify the number of times to repeat the modeled portion by increasing

the value of Number of Repeats. If, for example, you modeled a ° sector of a duct and you wanted

to display results on the entire duct, you would set Number of Repeats to .

In some cases, there may be multiple zones with different periodicity in the domain. For example, in

turbomachinery problems with multiple blade rows using the mixing plane model, the periodic angles

are different for each blade row. One blade may contain  blades (° periodic angle) and other may

contain  blades (° periodic angle). In such cases select the required cell zone and specify the

number of repeats for that particular cell zone.

When you click Set in the Graphics Periodicity Dialog Box (p. ) the graphics display will be immediately

updated to show the requested periodic repeats.

Figure . : Before Applying Periodicity (p. ) and Figure . : After Applying Periodicity (p. )

shows the display for the sample geometry before and after applying the periodic repeats respectively.

In this case the value of Number of Repeats is set to  for the ° sector (outer part) and to a value

of  is set for the ° sector (inner part) of the geometry.

Figure . : Before Applying Periodicity

Figure . : After Applying Periodicity

.... Periodic Repeats for Graphics

To define graphical periodicity for a non-periodic domain, do the following:

.

Click Define... under Periodic Repeats in the Views Dialog Box (p. ).

Figure . : The Graphics Periodicity Dialog Box

.

In the resulting Graphics Periodicity Dialog Box (p. ) (Figure . :The Graphics Periodicity Dialog

Box (p. )), select the Cell Zone for which you want to specify the number of repeats.

Associated Surfaces list contains the surfaces associated with the selected cell zone. This is only in-

formative and you cannot edit the selection of surfaces in this box.

.

Specify Rotational or Translational as the Periodic Type.

.

For translational periodicity, specify the Translation distance of the repeated domain in the X, Y, and

Z directions. For rotational periodicity, specify the axis about which the periodicity is defined and the

Angle by which the domain is rotated to create the periodic repeat. For 3D problems, the axis of rotation

is the vector passing through the specified Axis Origin and parallel to the vector from (,,) to the

(X,Y,Z) point specified under Axis Direction. For 2D problems, you will specify only the Axis Origin;

the axis of rotation is the -direction vector passing through the specified point.

.

Specify Number of Repeats for the selected cell zone.

.

Click Set in the Graphics Periodicity Dialog Box (p. ).

.

Follow the same procedure for other cell zones.

.

Click Apply in the Views Dialog Box (p. ) to visualize the modified display.

You can delete the definition of any periodicity you have defined for graphics by clicking Reset in

the Graphics Periodicity Dialog Box (p. ).

Note

For the 3D domain with multiple periodic zones having different periodicity, ANSYS Fluent

can repeat only mesh, contour and vector plots, and not the pathlines and particle tracks.

Also if such domain contains, isosurfaces and clip-surfaces, that are associated with a par-

ticular cell zone, they are repeated using the same periodicity that is defined for that cell

zone. However, if the surface is not associated with any cell zone, you cannot specify the

periodicity for that surface.

.... Mirroring for Graphics

To define a mirror plane for a non-symmetric domain, do the following:

.

Click Define Plane... under Mirror Planes in the Views Dialog Box (p. ).

Figure . : The Mirror Planes Dialog Box

.

In the resulting Mirror Planes Dialog Box (p. ) (Figure . :The Mirror Planes Dialog Box (p. )), set

the coefficients of X, Y, and Z and the Distance (of the plane from the origin) in the following equation

for the mirror plane:

(.)

.

Click Add to add the defined plane to the Mirror Planes list.When you are done creating mirror planes,

(.)

.

click OK.The newly defined plane(s) will now appear in the Mirror Planes list in the Views Dialog

Box (p. ).To include the mirroring in the display, select the plane(s) and click Apply, as described

above.

If you want to delete a mirror plane that you have defined, select it in the Mirror Planes list in the

Mirror Planes Dialog Box (p. ) and click Delete. When you click OK in this dialog box, the deleted

plane will be removed permanently from the Mirror Planes list in the Views Dialog Box (p. ).

Figure . : The Scene Description Dialog Box (p. ) allows you to create a more complex scene than

what you can create using Figure . : The Scene Dialog Box (p. ).

Once you have displayed some geometric objects (meshes, surfaces, contours, vectors, and so on) in

your graphics window, you may want to move them around and change their characteristics to increase

the effectiveness of the scene displayed. You can use the Scene Description Dialog Box (p. ) (Fig-

ure . : The Scene Description Dialog Box (p. )) and the Display Properties Dialog Box (p. ) (Fig-

ure . : The Display Properties Dialog Box (p. )) and Transformations Dialog Box (p. ) (Fig-

ure . : The Transformations Dialog Box (p. )), which are opened from within it, to rotate, translate,

and scale each object individually, as well as change the color and visibility of each object.

Figure . : The Scene Description Dialog Box

The Iso-Value Dialog Box (p. ) (Figure . : The Iso-Value Dialog Box (p. )), which is also opened

from within the Scene Description Dialog Box (p. ), enables you to change the isovalue of a selected

isosurface. The Pathline Attributes Dialog Box (p. ) (Figure . : The Pathline Attributes Dialog

Box (p. )) lets you set some pathline attributes. The ability to make geometric objects visible and in-

visible is especially useful when you are creating an animation (see Animating Graphics (p. )) because

it enables you to add or delete objects from the scene one at a time. The ability to change the color

and position of an object independently of the others in the scene is also useful for setting up animations,

as is the ability to change isosurface isovalues. You will find the features in the Scene Description Dialog

Box (p. ) useful even when you are not generating animations because they enable you to manage

your graphics window efficiently. The procedure for overlaying graphics, which uses the Scene Descrip-

tion dialog box, is described in Advanced Graphics Overlays (p. ). (Note that you cannot use the

Scene Description Dialog Box (p. ) to control XY plot and histogram displays.)

... Selecting the Object(s) to be Manipulated

... Changing an Object’s Display Properties

...Transforming Geometric Objects in a Scene

... Modifying Iso-Values

... Modifying Pathline Attributes

... Deleting an Object from the Scene

In order to manipulate the objects in the scene, you will begin by selecting the object or objects of

interest in the Names list in the Scene Description Dialog Box (p. ) (Figure . : The Scene Description

Advanced Scene Composition

Dialog Box (p. )). The Names list is a list of the geometric objects that currently exist in the scene

(including those that are presently invisible). If you select more than one object at a time, any operation

(transformation, color specification, and so on) will apply to all the selected objects. You can also select

objects by clicking on them in the graphics display using the mouse-probe button, which is, by default,

the right mouse button. (See Controlling the Mouse Button Functions (p. ) for information about

mouse button functions.) To deselect a selected object, simply click its name in the Names list.

When you select one or more objects (either in the Names list or in the display), the Type field will

report the type of the selected object(s). Possible types for a single object include mesh, surface,

contour, vector, path, and text (that is, annotation text). This information is especially helpful

when you need to distinguish two or more objects with the same name. When more than one object

is selected, the type displayed is Group.

properties of each geometric object in the scene. You can specify different colors for displaying the

edges and faces of a mesh object to show the underlying mesh (edges) when the faces of the mesh

are filled and shaded. You can also make a selected object temporarily invisible. If, for example, you

are displaying the entire mesh for a complicated problem, you can make objects visible or invisible to

display only certain boundary zones of the mesh without regenerating the mesh display using the

Mesh Display Dialog Box (p. ). You can also use the visibility controls to manipulate geometric objects

for efficient graphics display or for the creation of animations. These features, plus several others, are

available in the Display Properties Dialog Box (p. ) (Figure . : The Display Properties Dialog

Box (p. )).

Figure . : The Display Properties Dialog Box

To set the display properties described above, select one or more objects in the Names list in the

Scene Description Dialog Box (p. ) and then click Display... to open the Display Properties Dialog

Box (p. ) for that object or group of objects.

.... Controlling Visibility

There are several ways for you to control the visibility of an object. All visibility options are listed

under the Visibility heading in the Display Properties Dialog Box (p. ).

To make the selected object(s) invisible, turn off the Visible option.To “undo” invisibility, enable the

Visible option again.

To turn the effect of lighting for the selected object(s) on or off, use the Lighting check box.You can

choose to have lighting affect only certain objects instead of all of them. Note that if Lighting is turned

on for an object such as a contour or vector plot, the colors in the plot will not be exactly the same as

those in the colormap at the left of the display.

To toggle the filled display of faces for the selected mesh or surface object(s), use the Faces option.

Turning Faces on here has the same effect as turning it on for the entire mesh in the Mesh Display Dialog

Box (p. ).

To turn the display of outer edges on or off, use the Outer Faces option.This option is useful for displaying

both sides of a slit wall. By default, when you display a slit wall, one side will “bleed” through to the other.

When you turn off the Outer Faces option, the display of a slit wall will show each side distinctly as you

rotate the display.This option can also be useful for displaying two-sided walls (that is, walls with fluid or

solid cells on both sides).

To turn the display of interior and exterior edges of the geometric object(s) on or off, use the Edges option.

To turn the display of the outline of the geometric object(s) on or off, use the Perimeter Edges check

box.

To toggle the display of feature lines (described in Adding Features to an Outline Display (p. )), if any,

for the selected object(s), use the Feature Edges option.

To toggle the display of the lines (if any) in the geometric object(s), use the Lines check box. Pathlines,

line contours, and vectors are “lines”.

To toggle the display of nodes (if any) in the geometric object(s), use the Nodes check box.

Once you have set the appropriate display parameters, click Apply to update the graphics display.

.... Controlling Object Color and Transparency

The Display Properties Dialog Box (p. ) also lets you control an object’s color and how transparent

it is. All color and transparency options are listed under the Colors heading.

To modify the color of faces, edges, or lines in the selected object(s), choose face-color, edge-color, line-

color, or node-color in the Color drop-down list.The Red, Green, and Blue color scales will show the

RGB components of the face, edge or line color, which you can modify by moving the sliders on the color

scales.When you are satisfied with the color specification, click Apply to save it and update the display.

The ability to set the colors for faces and edges can be useful when you want to have a filled display for

the mesh or surface, but you also want to be able to see the mesh lines.You can achieve this effect by

specifying different colors for the faces and the edges.

To set the relative transparency of an object, select face-color in the Color drop-down list. Move the slider

on the Transparency scale and click Apply to update the graphics display. An object with a transparency

of  is opaque, and an object with a transparency of  is transparent. By specifying a high transparency

value for the walls of a pipe, for example, you will be able to see contours that you have displayed on

cross-sections inside the pipe.This feature is available on all platforms when the software  buffer is used

for hidden surface removal, but if your display hardware supports transparency, it will be more efficient

to use the hardware  buffer as the hidden surface method instead.You can select these methods in the

Display Options Dialog Box (p. ), as described in Modifying the Rendering Options (p. ).

Important

If you save a picture of a display with transparent surfaces, you should not set the File

Type in the Save Picture Dialog Box (p. ) to Vector.

When you are composing a scene in your graphics window, you might find it helpful to move a partic-

ular object from its original position or to increase or decrease its size. For example, if you have displayed

contours or vectors on cross-sections of an internal flow domain (such as a pipe), you might want to

translate these cross-sections so that they will appear outside of the pipe, where they can be seen and

interpreted more easily. Figure . : Velocity Vectors Translated Outside the Domain for Better View-

ing (p. ) shows such an example.

Figure . : Velocity Vectors Translated Outside the Domain for Better Viewing

You can also move an object by rotating it about the -,

, or -axis. If you want to display one object

more prominently than the others, you can scale its size. If your geometry is rotating or has rotational

symmetry, you can display the meridional view. All of these capabilities are available in the Transform-

ations Dialog Box (p. ) (Figure . : The Transformations Dialog Box (p. )).

Figure . : The Transformations Dialog Box

To perform the transformations described above, select one or more objects in the Names list in the

Scene Description Dialog Box (p. ) and then click Transform... to open the Transformations Dialog

....Translating Objects

To translate the selected object(s), enter the translation distance in each direction in the X, Y, and Z

real number fields under Translate. Note that you can check the domain extents in the Scale Mesh

Dialog Box (p. ) or the Iso-Surface Dialog Box (p. ). Translations are not cumulative, so you can

easily return to a known state. To return to the original position, simply enter  in all three real

number fields.

.... Rotating Objects

To rotate the selected object(s), enter the number of degrees by which to rotate about each axis in

the X, Y, and Z integer number fields under Rotate By. You can enter any value between

and

. By default, the rotation origin will be (,,). If you want to spin an object about its own origin,

or about some other point, specify the X, Y, and Z coordinates of that point under Rotate About.

Rotations are not cumulative, so you can easily return to a known state. To return to the original po-

sition, simply enter  in all three integer number fields under Rotate By.

.... Scaling Objects

To scale the selected object(s), enter the amount by which to scale in each direction in the X, Y, and

Z real number fields under Scale. To avoid distortion of the object’s shape, be sure to specify the

same value for all three entries. Scaling is not cumulative, so you can easily return to a known state.

To return the object to its original size, simply enter  in all three real number fields.

.... Displaying the Meridional View

To display the meridional view of the selected object(s), enable the Meridional option. This option

is available only for 3D models. It is applicable to cases with a defined axis of rotation and is especially

useful in turbomachinery applications.

The meridional transformation projects the selected entities onto a surface of constant angular co-

ordinate,

. The resultant projection thus lies in an ( ,

) plane where  is in the direction of the ro-

tation axis and  is normal to it. The value of  used for the projection is taken as that corresponding

to the minimum ( ,

) point of the entity.

You can use the ability to generate surfaces with intermediate values between two isosurfaces (with

different isovalues) to create snapshots of the results. If the surfaces have contours, vectors, or pathlines

displayed on them, ANSYS Fluent will generate and display contours, vectors, or pathlines on the inter-

mediate surfaces that it creates.

.... Steps for Modifying Iso-Values

You can modify an isosurface’s isovalue directly by selecting it in the Names list in the Scene Descrip-

tion Dialog Box (p. ) or indirectly by selecting an object displayed on the isosurface. Then click Iso-

Value... to open the Iso-Value Dialog Box (p. ) (Figure . : The Iso-Value Dialog Box (p. )) for

the selected object. Note that this button is available only if the geometric object selected in the

Names list is an isosurface or an object on an isosurface (contour on an isosurface, for example);

otherwise it is grayed out.

Figure . : The Iso-Value Dialog Box

In the Iso-Value Dialog Box (p. ), set the new isovalue in the Value field, and click Apply. Contours,

vectors, or pathlines that were displayed on the original isosurface will be displayed for the new iso-

value.

If you are creating animations of existing pathlines, you may want to change the number of steps used

in the computation of the pathlines. This enables you to animate pathlines advancing through the

domain. To do so, select the pathlines in the Names list in the Scene Description Dialog Box (p. )

and then click Pathlines... to open the Pathline Attributes Dialog Box (p. ) (Figure . : The Pathline

Attributes Dialog Box (p. )).

Figure . : The Pathline Attributes Dialog Box

In the Pathline Attributes Dialog Box (p. ), set the new maximum number of steps for pathline

computation (Max Steps). After you change the value and click Apply, the selected pathline will be

recomputed and redrawn.

If you are composing a complex scene with overlays and find that you no longer want to keep one of

the objects, it is possible to delete it without affecting any of the other objects in the scene. The ability

to delete individual objects is especially useful if you have overlays on and you generate an unwanted

object (for example, if you generate contours of the wrong variable). You can simply delete the un-

wanted object and continue your scene composition, instead of starting over from the beginning.

Note that it is also possible to make objects temporarily invisible, as described in Controlling Visibil-

ity (p. ).

ity (p. ).

Object deletion is performed in the Scene Description Dialog Box (p. ) (Figure . : The Scene De-

scription Dialog Box (p. )). To delete an object from the scene, select it in the Names list and then

click Delete Geometry. The selected name will disappear from the Names list, and the display will be

updated immediately.

ANSYS Fluent enables you to add a bounding frame around your displayed domain. You may also include

measure markings on the bounding frame to indicate the length, height, and/or width of the domain,

as shown in Figure . : Graphics Display with Bounding Frame (p. ).

To add a bounding frame to your display, you will follow the procedure below:

.

Click Frame Options... in the Scene Description Dialog Box (p. ) (Figure . :The Scene Description

Dialog Box (p. )) to open the Bounding Frame Dialog Box (p. ) (Figure . :The Bounding Frame

Figure . : The Bounding Frame Dialog Box

.

Under Frame Extents in the Bounding Frame Dialog Box (p. ), select Domain or Display to indicate

whether the bounding frame should encompass the domain extents or only the portion of the domain

that is shown in the display.

.

In the Axes portion of the Bounding Frame Dialog Box (p. ), specify the frame boundaries and meas-

urements to be shown in the display:

Indicate the bounding plane(s) (for example, the x-z and y-z planes shown in Figure . : Graphics

Display with Bounding Frame (p. )) to be displayed by clicking on the white square on the appropriate

plane of the box shown under the Axes heading.You can use any of the mouse buttons.The square

will turn red to indicate that the associated bounding plane will be displayed in the graphics window.

Specify where you would like to see the measurement annotations by clicking on the appropriate

edge of the box.The edge will turn red to indicate that the markings will be displayed along that edge

of the displayed geometry.

Important

If you have trouble determining which square or edge corresponds to which location

in your domain, you can easily find out by displaying one or two bounding planes to

get your bearings. You can then select the appropriate objects to obtain the final display.

.

Click Display to update the display with the current settings. If you are not satisfied with the frame, repeat

steps  and/or  and click Display again.

.

Once you are satisfied with the bounding frame that is displayed, click OK to close the Bounding Frame

Dialog Box (p. ) and save the frame settings for future displays.

.

in the Scene Description Dialog Box (p. ) and click Apply. If this option is not enabled, the bounding

box will appear only in the current display; it will not be redisplayed when you generate a new display

The bounding planes and axis annotations will appear in the Names list of the Scene Description

Dialog Box (p. ), and you can manipulate them in the same way as any other geometric object in

the display. For example, you can use the Display Properties Dialog Box (p. ) to change the face

color of a bounding plane or to make it transparent (see Changing an Object’s Display Properties (p. )).

To generate animations that progress from one static view of the graphics display to the next, you can

set up “key frames” (individual static images) using the Animate Dialog Box (p. ) (Figure . : The

Animate Dialog Box (p. )).

Results → Animations → Scene Animation

Edit...

Animating Graphics

Figure . : The Animate Dialog Box

You can compose a scene in the graphics window and define it as a single key frame. Then, modify the

scene by moving or scaling objects, making some objects invisible or visible, changing colors, changing

the view, or making other changes, and define the new scene as another key frame. ANSYS Fluent can

then interpolate smoothly between the two frames that you defined, creating a specified number of

intermediate frames.

Animation Definition Dialog Box (p. ) to set up the graphical displays that you want to use in the

animation. You can choose the type of display you want to animate by selecting it from the Animation

Object list or by creating a new animation object. For details on animating the solution, see Animating

the Solution (p. ). For more information on generating, displaying, and saving pathlines and particle

tracks, refer to Displaying Pathlines (p. ). See Displaying Results on a Sweep Surface (p. ) for inform-

ation about displaying the mesh, contours, or vectors on a surface that sweeps through the domain.

Note

"Key frame" animations created through the Animate dialog box are not compatible with

iso-surfaces.

... Creating an Animation

... Playing an Animation

... Saving an Animation

... Reading an Animation File

... Notes on Animation

You can define any number of key frames (up to ) to create your animation. By assigning the ap-

propriate numbers to the key frames, you provide the information ANSYS Fluent needs to create the

correct number of intermediate frames. For example, to create a simple animation that begins with a

front view of an object, moves to a side view, and ends with a rear view of the object, you would follow

the procedure outlined below:

.

Determine the number of frames that you want in the animation. For this example, consider the animation

to be  frames.

.

Determine the number of key frames that you need to specify. In this example, you will specify three:

one showing the front view, one showing the side view, and one showing the rear view.

.

Determine the appropriate key frame numbers to assign to the  specified frames. Here, the front view

will be specified as key frame , the side view will be key frame , and the rear view will be key frame

.

.

Compose the scenes for each view to be used as a key frame.You can use the Scene Description Dialog

Box (p. ) (see Advanced Scene Composition (p. )) and the Views Dialog Box (p. ) (see Modifying

.

the View (p. )) to modify the display, and any other dialog boxes or commands to create contours,

vectors, pathlines, and so on to be included in each scene. After you complete each scene, create the

appropriate key frame by setting the Frame number and clicking Add under Key Frames in the Animate

Dialog Box (p. ). For special considerations related to key frame definition, see Notes on Anima-

tion (p. ).

Important

Be sure to change the Frame number before clicking Add, or you will overwrite the

last key frame that you created.

You can check any of the key frames that you have created by selecting it in the Keys list. The

selected key frame will be displayed in the graphics window.

.

When you complete the animation, you can play it back as described in Playing an Animation (p. )

and/or save it as described in Saving an Animation (p. ).

.... Deleting Key Frames

If, during the creation of your animation, you want to delete one of the key frames that you have

defined, select the key frame in the Keys list and click Delete. If you want to delete all key frames

and start over again, click Delete All.

Once you have defined the key frames (as described in Creating an Animation (p. )) or read in a

previously created animation file (as described in Reading an Animation File (p. )), you can play back

the animation and ANSYS Fluent will interpolate between the frames that you specified to complete

the animation.

To play the animation once through from start to finish, click the “play” button under the Playback

heading in the Animate Dialog Box (p. ). (The buttons function in a way similar to those on a

standard video cassette player.“Play” is the second button from the right—a single triangle pointing

to the right.) To play the animation backwards once, click the “play reverse” button (the second from

the left—a single triangle point to the left). As the animation plays, the Frame scale shows the number

of the frame that is currently displayed, as well as its relative position in the entire animation. If, instead

of playing the complete animation, you want to jump to a particular key frame, move the Frame slider

bar to the desired frame number, and the frame corresponding to the new frame number will be dis-

Additional options for playing back animations are described below. Be sure to check Notes on Anim-

ation (p. ) as well for important notes about playing back animations.

You may sometimes want to play only one portion of a long animation. To do this, you can modify

the Start Frame and the End Frame under the Playback heading in the Animate Dialog Box (p. ).

For example, if your animation contains  frames, but you want to play only frames  to , you

can set Start Frame to  and End Frame to . When you play the animation, it will start at frame

and finish at frame .

...."Fast-Forwarding" the Animation

You can "fast-forward" or "fast-reverse" the animation by skipping some of the frames during playback.

To fast-forward the animation, set the Increment and click the fast-forward button. If, for example,

your Start Frame is , your End Frame is , and your Increment is , when you click the fast-forward

button (the last button on the right—two triangles pointing to the right), the animation will show

frames , , , , , ,  and . Clicking on the fast-reverse button (the first button on the left—two

triangles pointing to the left) will show frames , , ,....

of the reverse play buttons), select Auto Repeat in the Playback Mode drop-down list in the Animate

To play the animation back and forth continuously, reversing the playback direction each time, select

Auto Reverse in the Playback Mode drop-down list.

setting.

To stop the animation during playback, click the "stop" button (the square in the middle of the

the left (a left-pointing triangle with a vertical bar). Frame-by-frame playback enables you to freeze

the animation at points that are of particular interest.

Once you have created your animation, you can save it in any of the following formats:

Animation file containing the key frame descriptions

Picture files, each containing a frame of the animation

MPEG file containing each frame of the animation

.... Animation File

You can save the key frame definitions to a file that can be read back into ANSYS Fluent (see Reading

an Animation File (p. )) when you want to replay the animation. Since the animation file will contain

only the key frame definitions, you must be sure that you have a case and data file containing the

necessary surfaces and other information referred to by the key frame descriptions.

To write an animation file, select Key Frames in the Write/Record Format drop-down list in the An-

imate Dialog Box (p. ), and click Write.... In The Select File Dialog Box (p. ), specify the name of

the file and save it.

You can also generate a picture file for each frame in the animation. This feature enables you to save

your animation frames to picture files used by an external animation program such as ImageMagick.

To save the animation as a picture file, follow these steps:

.

Select Picture Files in the Write/Record Format drop-down list in the Animate Dialog Box (p. ).

.

If necessary, click Picture Options... to open the Save Picture Dialog Box (p. ) and set the appropriate

parameters for saving the picture files. (If you are saving picture files for use with ImageMagick, for ex-

ample, you may want to select the window dump format. See Window Dumps (Linux Systems

Only) (p. ) for details.) Click Apply in the Save Picture Dialog Box (p. ) to save your modified settings.

Important

Do not click Save... in the Save Picture Dialog Box (p. ). You will save the picture

files from the Animate Dialog Box (p. ) in the next step.

.

In the Animate Dialog Box (p. ), click Write.... In The Select File Dialog Box (p. ), specify the filename

and click OK to save the files. (See Window Dumps (Linux Systems Only) (p. ) for information about

specifying filenames that increment automatically as additional pictures are saved.) ANSYS Fluent will

replay the animation, saving each frame to a separate file.

It is also possible to save all of the frames of the animation in an MPEG file, which can be viewed

using an MPEG decoder such as mpeg_play. Saving the entire animation to an MPEG file will require

less disk space than storing the individual window dump files (using the picture method), but the

MPEG file will yield lower-quality images. To save the animation to an MPEG file, follow these steps:

.

Select MPEG in the Write/Record Format drop-down list in the Animate Dialog Box (p. ).

.

In the Animate Dialog Box (p. ), click Write.... In The Select File Dialog Box (p. ), specify the filename,

and click OK to save the files.

ANSYS Fluent replays the animation and saves each frame to a separate scratch file; it then

combines all of the files into a single MPEG file.

If you have saved the key frames defining an animation to an animation file (as described in Saving

an Animation (p. )), you can read that file back in at a later time (or in different session) and play

the animation. Before reading in an animation file, be sure that the current case and data contain the

surfaces and any other information that the key frame description refers to.

To read an animation file, click Read... in the Animate Dialog Box (p. ). In The Select File Dialog

Box (p. ), specify the name of the file to be read.

When you are creating and playing back animations, note the following:

For smoother animations, enable the Double Buffering option in the Display Options Dialog Box (p. )

(see Modifying the Rendering Options (p. )).This will reduce screen flicker during graphics updates.

When you are defining key frames, you must create all geometric objects that will be used in the animation

before you create any key frames.You cannot create a key frame using one set of geometric objects and

then generate a new geometry (such as a vector plot) and include that in another key frame. Create all

geometric objects first, and then use the Display Properties Dialog Box (p. ) to control the visibility of

the objects in each key frame (see Controlling Visibility (p. )).

A single animation sequence can contain up to  key frames.

When you play back an animation, the colormap used will be the one that is currently active, not the one

that was active during “recording.”

In addition to the many graphics tools already discussed, ANSYS Fluent also provides tools that enable

you to generate XY plots and histograms of solution, file, profile, and residual data. You can modify the

colors, titles, legend, and axis and curve attributes to customize your plots. The following sections describe

the XY and histogram plotting features in ANSYS Fluent.

... Plot Types

... XY Plots of Solution Data

... XY Plots of File Data

... XY Plots of Profiles

... XY Plots of Circumferential Averages

... XY Plot File Format

... Residual Plots

... Histograms

... Modifying Axis Attributes

... Modifying Curve Attributes

Data can be plotted in XY (abscissa/ordinate) form or histogram form. Each form is described below.

An XY (abscissa/ordinate) plot is a line and/or symbol chart of data. Virtually any defined variable or

function is accessible for this type of plot. Furthermore, you may read in an externally-generated data

file in order to compare your results with experimental data. You can also use the XY-plot facility to

plot out profile data, the residual histories of variables, or the time histories if you have a transient

problem.

ANSYS Fluent provides tools for controlling many aspects of the XY plot, including background color,

legend, and axis and curve attributes. Figure . : Sample XY Plot (p. ) shows a sample XY plot.

Figure . : Sample XY Plot

To differentiate the data being displayed, you can customize the pattern, color and weight of the

data lines and the shape, color, and size of the data markers.

When an XY plot is displayed in the graphics window, you can use the mouse-probe option, but all

other functions are inactive for XY plots. In addition, you can use any of the mouse buttons to move

and resize the legend box.

.... Histograms

A histogram plot is a bar chart of data. It is a representation of a frequency of distribution by means

of rectangles of widths representing class intervals and with areas proportional to the corresponding

frequencies. When a histogram plot is displayed in the graphics window, you can use the mouse-

probe, but all other functions are inactive for histogram plots. Figure . : Sample Histogram (p. )

shows a sample histogram.

Histogram and XY Plots

Figure . : Sample Histogram

See Histogram Reports (p. ) for information about printing histogram reports. For more information

on histogram plots, see Histograms (p. ).

You can produce a very sophisticated XY plot by using data from several zones, surfaces, or files and

modifying the axis and curve attributes. Using the capability for loading external data files, you can

create plots that compare your ANSYS Fluent results with data from other sources. To get further in-

formation about the solution, you can investigate the frequency of distribution of the data using a

histogram (see Histograms (p. )).

.... Steps for Generating Solution XY Plots

You can create an XY plot of solution data using the Solution XY Plot Dialog Box (p. ) (Fig-

ure . : The Solution XY Plot Dialog Box (p. )).

Named XY plot definitions can be saved for later use. See Creating and Using Contour Plot Definitions (p. )

for additional information on graphics object definitions.

Results → Plots → XY Plot

New...

Figure . : The Solution XY Plot Dialog Box

The basic steps for generating a solution XY plot are as follows:

.

Specify the variable(s) you are plotting:

To plot a variable on the y-axis as a function of position on the x-axis, enable the Position on X Axis

option and choose the variable to be plotted on the y-axis in the Y Axis Function drop-down list.

Select a category from the upper list and then choose the desired quantity in the lower list. For an

explanation of the variables in the list, see Field Function Definitions (p. ).

To plot a variable on the x-axis as a function of position on the y-axis, enable the Position on Y Axis

option and choose the variable to be plotted on the x-axis in the X Axis Function drop-down list.

To plot one variable as a function of another, turn off both the Position on X Axis and Position on

Y Axis options and select the variables to be plotted in the X Axis Function and Y Axis Function

drop-down lists.

.

Specify the plot direction:

To plot a variable as a function of position along a specified direction vector, select Direction Vector

in the X Axis Function or Y Axis Function drop-down list (whichever is the position axis), and specify

the components of the direction vector for plotting under Plot Direction.The position axis of the

plot is indicated by the selection of Position on X Axis or Position on Y Axis.The positions plotted

will have coordinate values that correspond to the dot product of the data coordinate vector with

the plot direction vector. For example, if you are plotting a variable at the pressure outlet of the

geometry shown in Figure . : Geometry Used for XY Plot (p. ), you would specify the Plot Dir-

ection vector (,,) since you are interested in how the variable changes as a function of x. Fig-

ure . : Data Plotted at Outlet Using a Plot Direction of (,,) (p. ) shows the resulting XY plot.

(If you specified (,,) as the plot direction, all variable values would be plotted at the same position

(see Figure . : Data Plotted at Outlet Using a Plot Direction of (,,) (p. )), because the y value

is the same at every point on the pressure outlet.)

It is also possible to plot a variable as a function of position along the length of a specified curvilinear

surface.The curvilinear surface must be piecewise linear and it cannot contain more than one closed

curve, such as a complete circle.To plot a variable in this way, select Curve Length in the X Axis

Function or Y Axis Function drop-down list (whichever is the position axis).Then specify the plot

direction along the surface: to plot the variable along the direction of increasing curve length, select

Default under Plot Direction; to plot the variable in the direction of decreasing surface length, select

Reverse.To check the direction in which the variable will be plotted along a surface, select the surface

in the Surfaces list and click Show under Plot Direction. ANSYS Fluent will display the selected surface

in the graphics window, marking the start of the surface with a blue dot and the end of the surface

with a red dot. ANSYS Fluent will also display arrows on the surface showing the direction in which

the variable will be plotted.

Note

When running the parallel version of ANSYS Fluent, Curve Length is only supported

when the curvilinear surface is contained within a single partition.

.

Choose the surface(s) on which to plot data in the Surfaces list. Note that if you are plotting a variable

as a function of position along the length of a curvilinear surface, you can select only one surface in the

Surfaces list.

.

Set any of the options described below, or modify the attributes of the axes or curves as described in

Modifying Axis Attributes (p. ) and Modifying Curve Attributes (p. ).

.

Click Plot to generate the XY plot in the active graphics window.

You can use any of the mouse buttons to annotate the XY plot (see Adding Text to the Graphics

Window (p. )) or move the plot legend from its default position in the upper left corner of the

Figure . : Geometry Used for XY Plot

Figure . : Data Plotted at Outlet Using a Plot Direction of (,,)

.... Options for Solution XY Plots

The options mentioned in Steps for Generating Solution XY Plots (p. ) include the following.

You can include data from an external file in the solution XY plot to compare your results with exper-

You can also choose node or cell values to be plotted, and save the plot data to a file.

..... Including External Data in the Solution XY Plot

To add external data to your XY plot for comparison with your results, you must first ensure that

any external data files are in the format described in XY Plot File Format (p. ). You can then load

the file(s) by clicking on the Load File... button and specifying the file(s) to be read in The Select

File Dialog Box (p. ). Once a file has been loaded, its title will appear in the File Data list. You can

choose the data file(s) to be included in your plot from the titles in this list.

To remove a file from the File Data list, select it and then click Free Data.

values are displayed. If you prefer to display the cell values, turn the Node Values option off. Node-

averaged data curves may be somewhat smoother than curves for cell values.

boundary zone surfaces will actually be the face values. These face values are more accurate, as face-

only functions are computed on the faces and not on the cells. For these face-only functions, the

cell values on postprocessing surfaces will display the values in the cell. For more information about

cell values, see Cell Values (p. ).

If you are displaying the XY plot to show the effect of a porous medium or 2D fan boundary, to

depict a shock wave, or to show any other discontinuities or jumps in the plotted variable, you

should use cell values; if you use node values in such cases, the discontinuity will be smeared by

the node averaging for graphics and will not be shown clearly in the plot.

..... Saving the Plot Data to a File

as described in XY Plots of File Data (p. ), or add it to a plot of solution data, as described above.

To save the plot data to a file, enable the Write to File option in the Solution XY Plot Dialog

Box (p. ). The Plot button will change to the Write... button. Clicking on the Write... button will

invoke The Select File Dialog Box (p. ), in which you can specify a name and save a file containing

the plot data. The format of this file is described in XY Plot File Format (p. ).

To sort the saved plot data in order of ascending x-axis value, enable the Order Points option in

the Solution XY Plot Dialog Box (p. ) before you click Write.... This option is available only when

the Write to File option is enabled.

You can produce XY plots using data contained in external files. The File XY Plot Dialog Box (p. )

enables you to display data read from external files in an abscissa/ordinate plot form. The format of

the plot file is described in XY Plot File Format (p. ).

.... Steps for Generating XY Plots of Data in External Files

You can create an XY plot of data contained in one or more external files using the File XY Plot Dialog

Box (p. ) (Figure . : The File XY Plot Dialog Box (p. )).

Results →

Plots →

File → Set Up...

Results →

Plots →

Figure . : The File XY Plot Dialog Box

The steps for generating a file XY plot are as follows:

.

Click Load... to select the file(s) you want to plot. Note that report files and .xy files are supported (see

XY Plot File Format (p. ) for information on the .xy file format).

As soon as the files are loaded, the curves (plots) are all added to the Curve Information list.

.

Select the X and Y variables that you want plotted (for a report definition file) and/or specify the data

sets you want plotted for an .xy file.

Selecting/de-selecting Y variables and Data Sets adds or removes them from the Curve Inform-

ation list.

.

Modify legend names as needed.To modify a legend name:

. Select a name in the Legend Names list.

. Enter the new name in the text entry box to the right of the Change Legend Entry button.

. Click Change Legend Entry.

.

You can control the appearance of the axes and curves by clicking Axes... or Curves....

.

Click Plot to generate an XY plot of the data listed in the Curve Information list.

ANSYS Fluent enables two options for generating XY plots of data related to boundary profiles. Using

the Plot Profile Data Dialog Box (p. ), you can plot the original data points from the profile file you

have read into ANSYS Fluent. Alternatively, you can plot the values assigned to the cell faces on the

boundary after the profile file has been interpolated, by using the Plot Interpolated Data Dialog

Box (p. ).

Important

Note that you must have valid data when trying to use the profile plotting options.

For more information about boundary profiles, see Profiles (p. ).

Box (p. ).

Important

.... Steps for Generating Plots of Profile Data

Once you have read a profile file, it is available for plotting by using the Plot Profile Data Dialog

Box (p. ).

Results →

Plots →

Profile Data → Set Up...

Figure . : The Plot Profile Data Dialog Box

The procedure for generating an XY plot of the original profile data is as follows:

.

Select one of the profiles you have read from the Profile selection list.

.

Select a field of the profile from the Y Axis Function selection list.

.

Choose a variable against which you want to plot the field data, and select it from the X Axis Function

selection list.The available variables will vary depending on the profile, and include x, y, z, r, and time.

.

Modify the attributes of the axes or curves as described in Modifying Axis Attributes (p. ) and Modi-

fying Curve Attributes (p. ).

.

Click Plot to generate an XY plot of the profile field data.

.... Steps for Generating Plots of Interpolated Profile Data

To interpolate a profile you must first read a profile file for the case, and select a profile field in a

boundary conditions dialog box (for example, the Velocity Inlet Dialog Box (p. )). After the flow

solution has been initialized, the cell face values of the boundary zone can be plotted by using the

Plot Interpolated Data Dialog Box (p. ).

Results →

Plots →

Interpolated Data → Set Up...

Figure . : The Plot Interpolated Data Dialog Box

The procedure for generating an XY plot of the interpolated data is as follows:

.

Results →

Plots →

.

Select a zone from the Zones selection list. Only the zones for which you have set a profile field as one

or more of the parameters will be available in this list.

.

Select a profile-related parameter of the zone from the Y Axis Function selection list.The name of the

parameter will be the same as that of the drop-down list in the boundary condition dialog box from

which the profile field was selected.

.

selection list.The available variables are x, y, and (for 3D cases) z.

.

.

Click Plot to generate an XY plot of the cell face values on the boundary.

You can also generate a plot of circumferential averages in ANSYS Fluent. This enables you to find the

against the radial or axial coordinate.

.... Steps for Generating an XY Plot of Circumferential Averages

You can generate an XY plot of circumferential averages in the radial direction using the circum-

avg-radial text command:

plot → circum-avg-radial

or you can use the circum-avg-axial text command to generate an average in the axial direction:

plot → circum-avg-axial

The procedure for generating an XY plot of circumferential averages is as follows:

.

Specify the variable to be averaged by typing its name when ANSYS Fluent prompts you for averages

of.You can press Enter to see a list of available variables.

.

Choose the surface on which to plot data by typing its name when ANSYS Fluent prompts you for on

surface.

Important

Use the Mesh Display Dialog Box (p. ) to see a list of surfaces on which you can

plot data. Pressing Enter will not show a list of available surfaces.

.

Specify the number of bands to be created.The default number of bands is .

ANSYS Fluent will create circumferential bands by isoclipping the specified surface into equal

bands of radial or axial coordinate. An example of the iso-clips created is shown in Figure . : Iso-

Clips Created For Circumferential Averaging (p. ). The radial or axial coordinate is derived from

the rotation axis of the Reference Zone specified in the Reference Values Task Page (p. ).

Figure . : Iso-Clips Created For Circumferential Averaging

ANSYS Fluent then computes the average of the variable for each band using the area-weighted av-

erage described in Computing Surface Integrals of the Theory Guide. Finally, it plots the average of

the variable as a function of radial or axial coordinate. Figure . : XY Plot of Circumferential Aver-

ages (p. ) shows an example of an XY plot of circumferential averages using radial coordinates.

Figure . : XY Plot of Circumferential Averages

When the circumferential average plot is generated, ANSYS Fluent also creates a new surface called

radial-bands or axial-bands, which contains the iso-clips described above (see Figure . : Iso-

Clips Created For Circumferential Averaging (p. )). You can use this surface to generate other XY

plots. For more information on the creation and manipulation of surfaces, see Creating Surfaces and

Cell Registers for Displaying and Reporting Data (p. ).

.... Customizing the Appearance of the Plot

If you want to customize the appearance of the axes or curves in a circumferential average plot, you

can save the plot data to a file (using the plot-to-file text command, as described in XY Plot

File Format (p. )), read the file into ANSYS Fluent and plot it again (using the File XY Plot Dialog

Box (p. ), as described in XY Plots of File Data (p. )), and then use the Axes Dialog Box (p. )

and Curves Dialog Box (p. ) (as described in Modifying Axis Attributes (p. ) and Modifying Curve

Attributes (p. )) to modify the appearance of the plot.

To save the plot data to a file, first use the plot-to-file text command to specify the name of

the file.

plot → file-set → plot-to-file

Then generate the circumferential average XY plot as described above. ANSYS Fluent will display the

plot in the graphics window, and also save the plot data to the specified file.

The XY file format read or written by ANSYS Fluent includes the following information:

The title of the plot

The label for the abscissa and the ordinate

Cortex variables and pairs of abscissa/ordinate data for each curve in the plot

The following sample file illustrates the XY file format:

(title "Velocity Magnitude")

(labels "Position" "Velocity Magnitude")

((xy/key/label "pressure-inlet-")

(xy/key/visible? #t)

(xy/line/pattern "--")

. . .

.

. .

...

. .

)

Similar to the case file format, parentheses bound the various pieces of information in the formatted,

ASCII file. The title (title " ") and labels (labels " ") must be first in the file, then each

curve has information in the form ((cxvar value) x y x y x y...), where there may be

zero or more Cortex variables defined for each curve.

You do not have to include Cortex variables to import your XY data. For example, you may want to

import experimental data to compare with the ANSYS Fluent solution. The following example would

use the default Cortex variables in the code to define the data. After you import the file into ANSYS

Fluent, you could then use the Axes Dialog Box (p. ) and the Curves Dialog Box (p. ) to customize

the XY plot, as described in Modifying Axis Attributes (p. ) and Modifying Curve Attributes (p. ).

(title "Experiment, Run ")

(labels "X, m" "Cp")

(  .

. .

. .

. .

)

Residual history can be displayed using an XY plot. The abscissa of the plot corresponds to the number

of iterations and the ordinate corresponds to the log-scaled residual values.

To plot the current residual history, click Plot in the Residual Monitors Dialog Box (p. ).

Edit...

For additional information about using the Residual Monitors Dialog Box (p. ) to plot residuals, see

Printing and Plotting Residuals (p. ).

Edit...

Histograms can be displayed in a graphics window using a bar chart (or printed in the console window,

as described in Histogram Reports (p. )). The abscissa of the chart is the desired solution quantity

and the ordinate is the percentage of the total number of cells.

.... Steps for Generating Histogram Plots

You can create a histogram plot of solution data using the Histogram Dialog Box (p. ) (Fig-

ure . : The Histogram Dialog Box (p. )).

Results → Plots → Histogram

Edit...

Figure . : The Histogram Dialog Box

The steps for generating a histogram plot are as follows:

.

Choose the scalar quantity to be plotted in the Histogram Of drop-down list. Select a category in the

upper list and then select the desired quantity in the lower list. (See Field Function Definitions (p. )

for an explanation of the variables in the list.)

.

Set the number of data intervals that will be plotted in the histogram in the Divisions field. By default

there will be  intervals (“bars”) in the histogram plot to finer intervals, increase the number of Divisions.

You may want to click Compute to update the Min and Max fields when you are trying to decide how

many divisions to plot.

.

Select the face or cell zone under Zones for which you want results plotted or printed. If all zones are

selected, then the entire domain will be plotted.You can also plot histograms based on the selected

Zone Types.

.

Set the option described below, if desired, or modify the attributes of the axes or curves as described

.

in Modifying Axis Attributes (p. ) and Modifying Curve Attributes (p. ).

.

Click Plot to generate the histogram plot in the active graphics window.

.

Click Print to print out your histogram results on individual zones, or the entire domain. Similarly, you

can click Compute to calculate your histogram results on individual zones, or the entire domain.

.... Options for Histogram Plots

Other than the axis and curve attribute controls mentioned in the procedure above, the only option

for histogram plotting is the ability to specify a subrange of values to be plotted.

..... Specifying the Range of Values Plotted

By default, the range of values included in the histogram plot is automatically set to the range of

values in the entire domain for the selected variable. If you want to focus in on a smaller range of

values, you can restrict the range to be displayed.

To manually set the range of values, turn off the Auto Range option in the Histogram Dialog

Box (p. ). The Min and Max fields will become editable, and you can enter the new range of values

to be plotted. To show the default range at any time, click Compute and the Min and Max fields

will be updated.

lected surfaces, rather than in the entire domain. To do this, turn off the Global Range option in

the Histogram Dialog Box (p. ). The Min and Max values will be updated when you next click

Compute.

You can modify the appearance of the XY and parameters that control the labels, scale, range, numbers,

Compute.

and major and minor rules. For each type of plot (solution XY, file XY, profile, residual, histogram, and

so on), you can set different axis parameters in the Axes Dialog Box (p. ) (Figure . : The Axes

Dialog Box (p. )). Note that the title following Axes in the dialog box indicates which plot environment

you are changing (for example, the Axes - Solution XY Plot dialog box controls parameters for solution

XY plots).

Figure . : The Axes Dialog Box

To open the Axes Dialog Box (p. ) for a particular plot type, click Axes... in the appropriate dialog

box (for example, the Solution XY Plot, File XY Plot, Plot Profile Data, Plot Interpolated Data, or

Residual Monitors dialog box).

.... Using the Axes Dialog Box

The Axes Dialog Box (p. ) enables you to independently control the characteristics of the ordinate

(y-axis) and abscissa (x-axis) on an XY plot or parameters for one axis or the other, by following the

procedure below:

.

Choose the axis for which you want to modify the attributes by selecting X or Y under Axis.

.

Set the desired parameters.

.

Click Apply and then choose the other axis and repeat the steps, if desired.

The changes to the axis attributes will appear in the graphics window the next time you generate a

plot.

..... Changing the Axis Label

If you want to modify the label for the axis, you can do so by editing the Label text field in the Axes

..... Changing the Format of the Data Labels

You can change the format of the labels that define the primary data divisions on the axes using

the controls under the Number Format heading in the Axes Dialog Box (p. ).

..... Choosing Logarithmic or Decimal Scaling

By default, decimal scaling is used for both axes (except for the -axis in residual plots, which uses

a log scale). If you want to change to a logarithmic scale, enable the Log option in the Axes Dialog

Box (p. ). To return to a decimal scale, turn off the Log option. Note that when you are using the

logarithmic scale, the Range values are the exponents; to specify a logarithmic range from  to

, for example, you will specify a minimum value of  and a maximum value of .

..... Resetting the Range of the Axis

By default, the extents of the axis will range from the minimum value plotted to the maximum value

plotted. If you want to change the range or extents of the axis, you can do so by turning off the

Auto Range option in the Axes Dialog Box (p. ) and setting the new Minimum and Maximum

values for the Range. This feature is useful when you are generating a series of plots and you want

the extents of one or both of the axes to be the same, even if the range of plotted values differs.

For example, if you are generating plots of temperature on several different wall zones, you might

want the minimum and maximum temperature on the -axis to be the same in every plot so that

you can easily compare one plot with another. You would determine a temperature range that in-

cludes the temperatures on all walls, and use that as the range for the -axis in each plot.

..... Controlling the Major and Minor Rules

ANSYS Fluent enables you to display major and/or minor rules on the axes. Major and minor rules

are the horizontal or vertical lines that mark, respectively, the primary and secondary data divisions

and span the whole plot window to produce a “mesh.” To add major or minor rules to the plot, enable

the Major Rules or Minor Rules option. You can then specify a color and weight for each type of

rule. Under the Major Rules or Minor Rules heading, select the desired color for the lines in the

Color drop-down list and specify the line thickness in the Weight field. A line of weight . is normally

pixel wide. A weight of . would make the line twice as thick (that is,  pixels wide).

The data curves in XY plots and histograms can be represented by any combination of lines and

markers. You can modify the attributes of the curves, including the patterns, weights, and colors of

the lines, and the symbols, sizes, and colors of the markers. For each type of plot (solution XY, file XY,

profile, residual, parameters in the Curves Dialog Box (p. ) (Figure . : The Curves Dialog Box (p. )).

Note that the title following Curves in the dialog box indicates which plot environment you are

changing (for example, the Curves - Solution XY Plot dialog box controls curve parameters for solution

XY plots).

Figure . : The Curves Dialog Box

To open the Curves Dialog Box (p. ) for a particular plot type, click Curves... in the appropriate

dialog box (for example, Solution XY Plot, File XY Plot, Plot Profile Data, Plot Interpolated Data,

or Residual Monitors dialog box).

.... Using the Curves Dialog Box

The Curves Dialog Box (p. ) enables you to independently control the characteristics of each data

curve in an XY plot or parameters for a curve, you will follow the procedure below:

.

Specify the curve for which you want to modify the attributes by increasing or decreasing the Curve #

counter.The curves are numbered sequentially, starting from . For example, if you were plotting flow-

field values on two surfaces, the first surface would be curve , and the second, curve . If the plot

contains only one curve, the Curve # is set to  and is not editable.

.

Set the desired line and/or marker parameters as described below.

.

Click Apply and then choose another Curve # and repeat the steps, if desired.

Your changes to the curve attributes will appear in the graphics window the next time you generate

a plot.

.

a plot.

..... Changing the Line Style

You can control the pattern, color, and weight of the line using the controls under the Line Style

heading:

To set the line pattern for the curve, choose one of the items in the Pattern drop-down list. Except for

center and phantom lines, the list displays examples of the pattern choices. A center line alternates a

very long dash and a short dash and a phantom line alternates a very long dash and a double short dash.

Note that selecting the second item in the drop-down list, represented by  short dashes, will result in

a solid-line curve.

Important

If you do not want the data points to be connected by any type of line (that is, if you

plan to use just markers), select the “blank” choice, which is the first item in the Pattern

list.

To set the color of the line, pick one of the choices in the Color drop-down list.

To define the line thickness, set the value of Weight. A line weight of . is normally  pixel wide.

Therefore, a weight of . would make the line twice as thick (that is,  pixels wide).

..... Changing the Marker Style

You can control the symbol, color, and size for the data marker using the controls under the Marker

Style heading:

To set the symbol used to mark data, choose one of the items in the Symbol drop-down list.The list

displays examples of the symbol choices. For example, in plotting pressure-coefficient data on the upper

and lower surfaces of an airfoil, the symbol /*\ (filled-in upward-pointing triangle) could be used for

the marker representing the upper surface data, and the symbol \*/ (filled-in downward-pointing triangle)

could be used for the marker representing the lower surface data.

Important

If you do not want the data points to be represented by markers (that is, if you plan

to use just a line connecting the data points), select the “blank” choice, which is the

first item in the Style list.

To set the color of the marker, pick one of the choices in the Color drop-down list.

To define the size of the data marker, set the value of Size. A symbol of size . is .% of the height of

the display screen, except for the “.” symbol, which is always one pixel.

..... Previewing the Curve Style

To see what a particular setting will look like in the plot, you can preview it in the Sample window

of the Curves Dialog Box (p. ). A single marker and/or line will be shown with the specified style

attributes.

In addition to the many graphics tools already discussed, ANSYS Fluent also provides turbomachinery-

specific postprocessing features that can be accessed once you have defined the topology of the

problem. Information on postprocessing for turbomachinery applications is provided in the following

sections:

... Defining the Turbomachinery Topology

... Generating Reports of Turbomachinery Data

... Displaying Turbomachinery Averaged Contours

... Displaying Turbomachinery 2D Contours

... Generating Averaged XY Plots of Turbomachinery Solution Data

... Globally Setting the Turbomachinery Topology

...Turbomachinery-Specific Variables

In order to establish the turbomachinery-specific coordinate system used in subsequent postprocessing

functions, ANSYS Fluent requires you to define the topology of the flow domain. The procedure for

defining the topology is described further in this section, along with details about the boundary types.

The current implementation of the turbomachinery topology definition for postprocessing is no longer

limited to one row of blades at a time. If your geometry contains multiple rows of blades, you can

define all turbomachinery topologies simultaneously. You can name and/or manage all topologies and

perform various turbomachinery postprocessing tasks on a single topology or on all topologies at

once.

Important

The turbo coordinates can only be generated properly if the correct rotation axis is specified

in the boundary conditions dialog box for the fluid zone (see Specifying the Rotation Ax-

is (p. )).

To define the turbomachinery topology in ANSYS Fluent, you will use the Turbo Topology Dialog

Box (p. ) (Figure . : The Turbo Topology Dialog Box (p. )).

Domain → Mesh Models → Turbo Topology...

Turbomachinery Postprocessing

Figure . : The Turbo Topology Dialog Box

The procedure for defining topology for your turbomachinery application are as follows:

.

Select a boundary type under Boundaries (for example, Hub in Figure . :The Turbo Topology Dialog

Box (p. )).The boundary types are described in detail in Boundary Types (p. ).

.

In the Surfaces list, choose the surface(s) that represent the boundary type you selected in step .

.

.

Repeat the steps  and  for all the boundary types that are relevant for your model.

Important

For a complete turbo topology definition the surfaces defined as inlet, outlet, hub,

casing, periodic, theta min, and theta max (if available) should form a closed domain.

.

Enter a name in the Turbo Topology Name field or keep the default name.

.

Click Define to complete the definition of the boundaries.

ANSYS Fluent will inform you that the turbomachinery postprocessing functions have been activ-

ated.

.

Specify a position vector that is defined as

.This position vector should be outside the domain, for

example, if your domain lies in the first and second quadrant, specify negative -axis as the zero  line.

This will ensure that there is no discontinuity in angular coordinates within the domain.This can be done

using the display/set/zero-angle-dir command.

Default zero

line is

axis. If this axis passes through the domain, you should define the zero

line, so as to satisfy above criteria.

.

To view a defined topology, select the topology from the Turbo Topology Name drop-down list and

.

click Display.The defined topology is shown in the active graphics window.This enables you to visually

check the boundaries to ensure that you have defined them correctly.

.

To edit a defined topology, select the topology from the Turbo Topology Name drop-down list, make

the appropriate changes and click Modify.

.

To remove a defined topology, select the topology from the Turbo Topology Name drop-down list and

click Delete.

Important

Note that the topology setup that you define will be saved to the case file when you save

the current model. Thus, if you read this case back into ANSYS Fluent, you do not need to

set up the topology again.

However, use of a boundary condition file to set the turbo topology for two similar cases may not

work properly. In that case you need to set the turbo topology manually.

.... Boundary Types

The boundaries for the turbomachinery topology are as follows (see Figure . : Turbomachinery

Boundary Types (p. )):

Hub

is the wall zone(s) forming the lower boundary of the flow passage (generally toward the axis of rotation

of the machine).

Casing

is the wall zone(s) forming the upper boundary of the flow passage (away from the axis of rotation of

the machine).

Theta Periodic

is the periodic boundary zone(s) on the circumferential boundaries of the flow passage.

Theta Min

and Theta Max are the wall zones at the minimum and maximum angular ( ) positions on a circumfer-

ential boundary.

Inlet

is the inlet zone(s) through which the flow enters the passage.

Outlet

is the outlet zone(s) through which the flow exits the passage.

Blade

Inlet

Outlet

Blade

is the wall zone(s) that defines the blade(s) (if any). Note that these zones cannot be attached to the

circumferential boundaries. For this situation, use Theta Min and Theta Max to define the blade.

Figure . : Turbomachinery Boundary Types

Once you have defined your turbomachinery topologies, as described in Defining the Turbomachinery

Topology (p. ), you can report a number of turbomachinery quantities, including mass flow, swirl

number, torque, and efficiencies.

To report turbomachinery quantities in ANSYS Fluent, you will use the Turbo Report Dialog Box (p. )

(Figure . : The Turbo Report Dialog Box (p. )).

Results → Model Specific → Turbo Topology → Report...

Figure . : The Turbo Report Dialog Box

The procedure for using this dialog box is as follows:

.

Under Averages, specify whether you want to report Mass-Weighted or Area-Weighted averages.

.

Under Turbo Topology, specify a predefined turbomachinery topology from the drop-down list.

.

Click Compute. ANSYS Fluent will compute the turbomachinery quantities as described below, and display

their values.

.

If you want to save the reported values to a file, click Write... and specify a name for the file in The Select

.... Computing Turbomachinery Quantities

..... Mass Flow

The mass flow rate through a surface is defined as follows:

(.)

where

= is the area of the inlet or outlet

= the velocity vector

= the fluid density

= a unit vector normal to the surface

..... Swirl Number

(.)

where

The swirl number is defined as follows:

(.)

where

= the radial coordinate (specifically, the radial distance from the axis of rotation)

= the tangential velocity

= a unit vector normal to the surface,

= the inlet or outlet

..... Average Total Pressure

The area-averaged total pressure is defined as follows:

(.)

where

is the total pressure and  is the area of the inlet or outlet.

The mass-averaged total pressure is defined as follows:

(.)

where,

= the total pressure

= the area of the inlet or outlet

..... Average Total Temperature

The area-averaged total temperature is defined as follows:

(.)

where

is the total temperature and  is the area of the inlet or outlet.

The mass-averaged total temperature is defined as follows:

(.)

where,

= the total temperature

..... Average Flow Angles

The area-averaged flow angles are defined as follows:

(.)

in the radial direction, and

(.)

in the tangential direction, where

,

, and

represent the axial, radial, and tangential velocities,

The mass-averaged flow angles are defined as follows:

(.)

(.)

in the tangential direction.

..... Passage Loss Coefficient

The engineering loss coefficient is defined as follows:

(.)

where,

= the mass-averaged total pressure at the inlet

(.)

where,

= the mass-averaged total pressure at the outlet

= the density of the fluid

= the mass-averaged velocity magnitude at the inlet

The normalized loss coefficient is defined as follows:

(.)

where

is the mass-averaged static pressure at the outlet.

..... Axial Force

The axial force on the rotating parts is defined as follows:

(.)

where,

= the surfaces comprising all rotating parts

= the total stress tensor (pressure and viscous stresses)

= a unit vector parallel to the axis of rotation

.....Torque

The torque on the rotating parts is defined as follows:

(.)

where,

= the total stress tensor

= the position vector

..... Efficiencies for Pumps and Compressors

The definitions of the efficiencies for compressible and incompressible flows in pumps and com-

pressors are described in this section. Efficiencies for turbines are described later in this section.

Consider a pumping or compression device operating between states  and  as illustrated in Fig-

ure . : Pump or Compressor (p. ). Work input to the device is required to achieve a specified

compression of the working fluid.

Figure . : Pump or Compressor

Assuming that the processes are steady state, steady flow, and that the mass flow rates are equal

at the inlet and outlet of the device (no film cooling, bleed air removal, and so on), the efficiencies

for incompressible and compressible flows are as described in the following subsections.

...... Incompressible Flows

For devices such as liquid pumps and fans (2D boundaries or 3D cell zones) at low speeds, the

working fluid can be treated as incompressible. The efficiency of a pumping process with an incom-

pressible working fluid is defined as the ratio of the head rise achieved by the fluid to the power

supplied to the rotor/impeller. This can be expressed as follows:

(.)

where,

= volumetric flow rate

= net torque acting on the rotor/impeller

= rotational speed

This definition is sometimes called the “hydraulic efficiency”. Often, other efficiencies are included

to account for flow leakage (volumetric efficiency) and mechanical losses along the transmission

system between the rotor and the machine providing the power for the rotor/impeller (mechanical

efficiency). Incorporating these losses then yields a total efficiency for the system.

...... Compressible Flows

For gas compressors that operate at high speeds and high pressure ratios, the compressibility of the

working fluid must be taken into account. The efficiency of a compression process with a compressible

working fluid is defined as the ratio of the work required for an ideal (reversible) compression process

to the actual work input. This assumes the compression process occurs between states  and  for

a given pressure ratio. In most cases, the pressure ratio is the total pressure at state  divided by the

total pressure at state . If the process is also adiabatic, then the ideal state at  is the isentropic state.

From the foregoing definition, the efficiency for an adiabatic compression process can be written

as

(.)

where,

= total enthalpy at

= actual total enthalpy at

= isentropic total enthalpy at

If the specific heat is constant, Equation . (p. ) can also be expressed as

(.)

where,

= total temperature at

= actual total temperature at

= isentropic total temperature at

Using the isentropic relation

(.)

where  is the ratio of specific heats specified in the Reference Values Task Page (p. ).

The efficiency can be written in the compact form

(.)

Note that this definition requires data only for the actual states  and .

Compressor designers also make use of the polytropic efficiency when comparing one compressor

with another. The polytropic efficiency is defined as follows:

(.)

..... Efficiencies for Turbines

Consider a turbine operating between states  and  in Figure . : Turbine (p. ). Work is extracted

from the working fluid as it expands through the turbine. Assuming that the processes are steady

state, steady flow, and that the mass flow rates are equal at the inlet and outlet of the device (no

film cooling, bleed air removal, and so on), turbine efficiencies for incompressible and compressible

flows are as described below.

Figure . : Turbine

The efficiency of a turbine with an incompressible working fluid is defined as the ratio of the work

delivered to the rotor to the energy available from the fluid stream. This ratio can be expressed as

follows:

(.)

where,

follows:

(.)

where,

Note the similarity between this definition and the definition of incompressible compression efficiency

(Equation . (p. )). As with hydraulic pumps and compressors, other efficiencies (for example,

volumetric and mechanical efficiencies) can be defined to account for other losses in the system.

For high-speed gas turbines operating at large expansion pressure ratios, compressibility must be

accounted for. The efficiency of an expansion process with a compressible working fluid is defined

as the ratio of the actual work extracted from the fluid to the work extracted from an ideal (reversible)

process. This assumes that the expansion process occurs between states  and  for a given pressure

ratio. In contrast to the compression process, the pressure ratio for expansion is the total pressure

at state  divided by the total pressure at state . If the process is also adiabatic, then the ideal state

at  is the isentropic state.

From the foregoing definition, the efficiency for an adiabatic expansion process through a turbine

can be written as

(.)

where

(.)

where

(.)

the expansion efficiency can be written in the compact form

(.)

(.)

(.)

As with compressors, one may also define a polytropic efficiency for turbines. The polytropic efficiency

(.)

Turbo averaged contours are generated as projections of the values of a variable averaged in the cir-

cumferential direction and visualized on an -  plane. A sample plot is shown in Figure . : Turbo

Averaged Filled Contours of Static Pressure (p. ).

.... Steps for Generating Turbomachinery Averaged Contour Plots

You can display contours using the Turbo Averaged Contours Dialog Box (p. ) (Figure . : The

Turbo Averaged Contours Dialog Box (p. )).

Results → Model Specific → Turbo Topology → Averaged Contours...

Figure . : The Turbo Averaged Contours Dialog Box

The basic steps for generating a turbo averaged contour plot are as follows:

.

Select All or a specific predefined turbomachinery topology from the Turbo Topology drop-down list.

.

Select the variable or function to be displayed in the Contours of drop-down list. First select the desired

category in the upper list; you may then select a related quantity in the lower list. (See Turbomachinery-

Specific Variables (p. ) for a list of turbomachinery-specific variables, and see Field Function Defini-

tions (p. ) for an explanation of the variables in the list.)

.

Specify the number of contours in the Levels field.The maximum number of levels allowed is .

.

Set any of the options described below.

.

Click Display to draw the specified contours in the active graphics window.

.

.

The resulting display will include the specified number of contours of the selected variable, with the

magnitude on each one determined by equally incrementing between the values shown in the Min

and Max fields.

Note that the Min and Max values displayed in the dialog box are the minimum and maximum aver-

aged values. These limits will in general be different from the global Domain Min and Domain Max,

which are also displayed for your reference (see Figure . : The Turbo Averaged Contours Dialog

Box (p. )).

Figure . : Turbo Averaged Filled Contours of Static Pressure

.... Contour Plot Options

The options mentioned in the procedure above include drawing color-filled contours (instead of line

contours), specifying a range of values to be contoured, and storing the contour plot settings. These

options are the same as those in the standard Contours Dialog Box (p. ). See Contour and Profile

Plot Options (p. ) for details about using them.

In postprocessing a turbomachinery solution, it is often desirable to display contours on surfaces of

constant spanwise coordinate, and then project these contours onto a plane. This permits easier

evaluation of the contours, especially for surfaces that are highly three-dimensional.

.... Steps for Generating Turbo 2D Contour Plots

You can display contours using the Turbo 2D Contours Dialog Box (p. ) (Figure . : The Turbo

2D Contours Dialog Box (p. )).

Results → Model Specific → Turbo Topology → 2D Contours...

Figure . : The Turbo 2D Contours Dialog Box

The basic steps for generating a turbo 2D contour plot are as follows:

.

Specify a specific predefined turbomachinery topology using the Turbo Topology drop-down list.

.

Enter a value for the Normalized Spanwise Coordinates ( to ) for the spanwise surface you want

to create.

Important

If shroud and hub are the curved surfaces, the isosurface very close to them may

contain void spaces as ANSYS Fluent displays only a plane cut surface.

.

Select the variable or function to be displayed in the Contours of drop-down list.

First select the desired category in the upper list; you may then select a related quantity in the

lower list. See Turbomachinery-Specific Variables (p. ) for a list of turbomachinery-specific

variables, and see Field Function Definitions (p. ) for an explanation of the variables in the list.

.

.

Depending on the type of contour plot you want to display, select appropriate choice under Options.

These options are the same as those in the standard Contours Dialog Box (p. ). See Contour and

Profile Plot Options (p. ) for details about using them.

When comparing numerical solutions of turbomachinery problems to experimental data, it is often

useful to plot circumferentially averaged quantities in the spanwise and meridional directions. This

section describes how to do this in ANSYS Fluent.

.... Steps for Generating Turbo Averaged XY Plots

To create an XY plot of circumferentially averaged solution data, you will use the Turbo Averaged XY

Plot Dialog Box (p. ) (Figure . : The Turbo Averaged XY Plot Dialog Box (p. )).

Results → Model Specific → Turbo Topology → Averaged XY Plot...

Figure . : The Turbo Averaged XY Plot Dialog Box

The procedure for generating a turbo averaged XY plot are as follows:

.

Select the variable or function to be plotted in the Y Axis Function drop-down list. First select the desired

.

.

Select the variable or function to be plotted in the X Axis Function drop-down list.The choices are

Hub to Casing Distance and Meridional Distance.

.

Specify the desired value in the Fractional Distance field.The definition of the fractional distance de-

pends on your selection of X Axis Function:

If you select Hub to Casing Distance, the fractional distance will be Inlet to Outlet.

If you select Meridional Distance, the fractional distance will be Hub to Casing.

.

.

(optional) Modify the attributes of the axes or curves as described in Modifying Axis Attributes (p. )

and Modifying Curve Attributes (p. ).

.

Note that you can use any of the mouse buttons to annotate the XY plot (see Adding Text to

the Graphics Window (p. )).

If you want to write the XY data to a file, follow these steps instead of Step  above:

.

Enable the Write to File option.The Plot button changes to a Write... button.

.

Click Write....

.

In The Select File Dialog Box (p. ), specify a name for the plot file and save it.

In some cases, that is, isosurface creation, ANSYS Fluent enables you to globally set the current tur-

bomachinery topology for your model using the Turbo Options Dialog Box (p. ) (Figure . : The

Turbo Options Dialog Box (p. )).

Results → Model Specific → Turbo Topology → Options...

Figure . : The Turbo Options Dialog Box

To set the current topology, select a topology from the Current Topology drop-down list and select

OK.

The following turbomachinery-specific variables are available in ANSYS Fluent:

Meridional Coordinate

Abs Meridional Coordinate

Spanwise Coordinate

Abs (H-C) Spanwise Coordinate

Abs (C-H) Spanwise Coordinate

Pitchwise Coordinate

Abs Pitchwise Coordinate

These variables are contained in the Mesh... category of the variable selection drop-down list. See

Field Function Definitions (p. ) for their definitions.

When interpreting time-sequence data from a transient solution, it is often useful to look at the data’s

spectral (frequency) attributes. For instance, you may want to determine the major vortex-shedding

frequency from the time-history of the drag force on a body recorded during an ANSYS Fluent simulation.

Or, you may want to compute the spectral distribution of static pressure data recorded at a particular

location on a body surface. Similarly, you may need to compute the spectral distribution of turbulent

kinetic energy using data for fluctuating velocity components. To interpret some of these time dependent

data, you need to perform Fourier transform analysis. In essence, the Fourier transform enables you to

take any time dependent data and resolve it into an equivalent summation of sine and cosine waves.

ANSYS Fluent enables you to analyze your time dependent data using the Fast Fourier Transform (FFT)

algorithm. Information on using the FFT algorithm in ANSYS Fluent is provided in the following sections:

... Limitations of the FFT Algorithm

...Windowing

... Fast Fourier Transform (FFT)

... Using the FFT Utility

The following limitations apply to ANSYS Fluent’s FFT module:

The ANSYS Fluent FFT module can only read inputs files in the ANSYS Fluent report file, monitor, and x-y

file formats.

The ANSYS Fluent FFT module assumes that the input data have been sampled at equal intervals and are

consecutive (in the order of increasing time).

The lowest frequency that the FFT module can pick up is given by

, where  is the total sampling time.

If the sampled sequence contains frequencies lower than this, these frequencies will be aliased into higher

frequencies.

The highest frequency that the FFT module can pick up is

, where

is the sampling interval (or

time step).

The discrete FFT algorithm is based on the assumption that the time-sequence data passed to the FFT

corresponds to a single period of a periodically repeating signal. Since, in most situations, the first and

the last data points will not coincide, the repeating signal implied in the assumption can often have

a large discontinuity. The large discontinuity produces high-frequency components in the resulting

Fourier modes, causing an aliasing error. You can condition the input signal before the transform by

“windowing” it, in order to avoid this problem.

Suppose that we have

consecutive discrete (time-sequence) data sampled with a constant interval,

:

(.)

Windowing is done by multiplying the original input data (

) by a window function,

:

(.)

ANSYS Fluent offers four different window functions:

Hamming’s window:

(.)

Hanning’s window:

(.)

Barlett’s window:

(.)

Blackman’s window:

(.)

These window functions preserve a large fraction (

) of the original data, affecting only

of

the data on both ends.

The Fourier transform utility in ANSYS Fluent enables you to compute the Fourier transform of a signal,

, a real-valued function, from a finite number of its sampled points.

For a periodic set of

sampled points,

, the discrete Fourier transform [] (p. ) expresses the

signal as a finite trigonometric series:

(.)

where the series coefficients

are computed as

Fast Fourier Transform (FFT) Postprocessing

(.)

Equation . (p. ) and Equation . (p. ) form a Fourier transform pair that enables us to de-

termine one from the other.

Note that when we follow the convention of varying  from  to

Equation . (p. ) instead of from

to

, the range of index

corresponds

to positive frequencies, and the range of index

corresponds to negative frequencies.

still corresponds to zero frequency.

For the actual calculation of the transforms, ANSYS Fluent adopts the so-called fast Fourier transform

(FFT) algorithm, which significantly reduces operation counts in comparison to the direct transform.

Furthermore, unlike most FFT algorithms in which the number of data should be a power of , the

FFT utility in ANSYS Fluent employs a prime-factor algorithm  [] (p. ). The number of data points

permissible in the prime-factor FFT algorithm is any products of mutually prime factors from the set

, with a maximum value of

. Thus, the prime-factor

FFT preserves the original data better than the conventional FFT.

Just prior to computing the transform, ANSYS Fluent determines the largest permissible number of

data points based on the prime factors, discarding the rest of the data. A list of these numbers is

provided in Table . : Numbers of Data Points Supported by the Prime-Factor FFT Algorithm (p. ).

Table . : Numbers of Data Points Supported by the Prime-Factor FFT Algorithm

The ANSYS Fluent FFT utility is available through the Fourier Transform Dialog Box (p. ) (Fig-

ure . : The Fourier Transform Dialog Box (p. )).

Results →

Plots →

FFT → Set Up...

Figure . : The Fourier Transform Dialog Box

.... Loading Data for Spectral Analysis

FFT analysis requires an input signal data file consisting of time-sequence data. To load an input signal

data file into the Fourier Transform Dialog Box (p. ), click Load Input File.... This displays The Select

File Dialog Box (p. ) where you can browse through your file directories and locate your data file

containing your time-sequence data. To remove a file from the Files list, select it and then click Free

File Data.

If you computed acoustic signals “on the fly”, you have the option of processing signal data from a

file or processing receiver data stored in memory. To analyze signal data from an existing input file,

select Process File Data under Process Options and proceed as described above. To analyze receiver

data stored in memory, select Process Receiver under Process Options and select the appropriate

receiver in the Receiver list.

Click Plot FFT to display the spectral analysis data and, if you have enabled Acoustics Analysis, to

calculate the overall sound pressure level in dB based on the Reference Acoustic Pressure and display

it in the console.

Note

Note

You can specify the  axis and  axis variables if your input report file contains multiple

report definitions.

.... Customizing the Input and Defining the Spectrum Smoothing

With the input signal data file loaded into the Fourier Transform Dialog Box (p. ), you may want

to view a plot of the input signal and/or customize the data set in preparation for applying the FFT

algorithm. To do so, click the Plot/Modify Input Signal button to open the Plot/Modify Input Signal

Dialog Box (p. ) (Figure . : The Plot/Modify Input Signal Dialog Box (p. )).

Figure . : The Plot/Modify Input Signal Dialog Box

The Plot/Modify Input Signal Dialog Box (p. ) allows you to analyze a portion of the input signal,

view input Signal Statistics—Min, Max, Mean, Variance, total Number of Samples, and Min Fre-

quency (that is, the finest possible frequency resolution)—and set title and label information for the

input signal plot. Additionally, this dialog box allows you to enable and control the smoothing of the

resulting spectrum by subdividing the input signal into multiple segments and averaging the segment-

based spectra.

Note

..... Customizing the Input Signal Data Set

By default, the entire data set is analyzed. To analyze a portion of the input signal, enable the Clip

to Range option and specify the data range by entering Min and Max values under X Axis Range.

To have the -axis quantities reduced by the Mean value of the relevant signal property, enable

the Subtract Mean Value option.

The Set Defaults button will reset the original values for the Min and Max fields under X Axis Range

and turn off the Clip to Range option.

..... Spectrum Smoothing Through Signal Segmentation

For long broadband noise signals, the computed Fourier spectrum may display spurious fluctuations

of amplitudes between the neighboring modes. In order to obtain a smooth spectrum, you can split

the signal into multiple overlapping segments so that ANSYS Fluent can apply the FFT algorithm on

each segment and then average the resulting spectra. This procedure allows you to significantly

suppress the spurious fluctuations at the cost of coarsening the frequency resolution of the spectrum.

Note that the arithmetic averaging of spectra is performed for the squares of Fourier amplitudes,

thus conserving the signal energy.

To use the smoothing procedure, enable the Subdivide into Segments option and define the seg-

ment size and the overlap of the subsequent segments in the Segment Control group box. Make

a selection from the Control Method list to specify how you want to define the segment size: select

Samples if you want to specify the number of Samples per Segment; select Frequency if you want

to specify the desired Frequency Resolution

in Hertz units (the segment length in seconds is

then equal to

). To help determine a suitable segment size, you can use the Number of

Samples and the Min Frequency information in the Signal Statistics group box. Note that the final

segment length is selected by ANSYS Fluent to adhere to the largest supported number of data

samples (see Table . : Numbers of Data Points Supported by the Prime-Factor FFT Algorithm (p. )).

The actual signal length and the number of segments will be displayed in the console when you

plot or write the Fourier spectrum. The number of segments depends on the Overlap of the sub-

sequent segments, which is specified regardless of which Control Method you select. If you select

a Window function (see Windowing (p. ) for details), it is recommended that you use an Overlap

value of at least ., in order to cover the signal portion affected by the window function. Generally,

an Overlap value of . is recommended. The exact number of samples that are in the overlapping

region of the segment can be determined from the segment hop size, which is displayed in the

console. The segment hop size is the distance (in terms of samples) between the starting samples

of any two adjacent segments (that is, the shift from one segment to the next), and has a minimum

value of .

The Set Defaults button will reset the segment control values and disable the Subdivide into

Segments option.

.....Viewing Data Statistics

To aid in the signal analysis, whether for the entire input signal or for a certain range of data, the

Signal Statistics group box in the Plot/Modify Input Signal Dialog Box (p. ) displays signal inform-

ation such as the minimum, maximum, and average signal values, as well as the signal variance,

total number of samples, and finest possible frequency resolution.

..... Customizing Titles and Labels

You can create a new title or edit the original title for the input signal plot by entering a text string

in Signal Plot Title. Likewise, you can create a new axis label or edit the original axis label by entering

a text string into either Y Axis Label or X Axis Label.

..... Applying the Changes in the Input Signal Data

To apply any changes you have made in the Plot/Modify Input Signal Dialog Box (p. ) and view

a plot of the input signal, click Apply/Plot.

.... Customizing the Output

In most practical applications with CFD data, you may want to find out how much power or energy

is contained in a certain frequency range, but do not want to distinguish positive and negative fre-

quency. In recognition of this, all the outputs from the FFT module in ANSYS Fluent pertain to one-

sided spectra for the range of positive frequency.

The Fourier Transform Dialog Box (p. ) (Figure . : The Fourier Transform Dialog Box (p. )) and

Plot/Modify Input Signal Dialog Box (p. ) (Figure . : The Plot/Modify Input Signal Dialog

Box (p. )) enable you to set several different functions for the  and  axes, apply different FFT

windowing techniques, and set various output options.

..... Specifying a Function for the Y Axis

You can choose the -axis function using the Y Axis Function drop-down list. Available options for

the -axis functions are as follows. Note that the functions related to acoustics (all of which are

measured in dB) are only available when the Acoustics Analysis option is enabled.

The definitions are provided for

, and include contributions from both elements of a complex

conjugate pair  and

. Note that in ANSYS Fluent, the value of

is always an even number.

Power Spectral Density

is the distribution of signal power in the frequency domain. Its value and units depend on the X Axis

Function choice. For the detailed spectral representation with all resolved harmonics (that is, when X

Axis Function is either Frequency, Strouhal Number, or Fourier Mode), the Power Spectral Density

(

) has units of the signal magnitude squared over the frequency (for example, Pa2/Hz) and is defined

for the frequency

as

(.)

where

is the frequency step in the discrete spectrum, and the Fourier mode power

(.)

For the octave analysis (that is, when the X Axis Function is either Octave Band or /-Octave

Band), the Power Spectral Density has units of the signal magnitude squared (for example,

Pa2), and is defined for the frequency band

as

(.)

where  includes all of the Fourier modes belonging to the band.

Magnitude

is the amplitude. For the detailed spectral representation with all resolved harmonics (that is, when X

Axis Function is either Frequency, Strouhal Number, or Fourier Mode), the Magnitude ( ) is defined

as

(.)

where

is the mean signal value.

Band), the Magnitude is defined for the frequency band

as

(.)

where

is calculated according to Equation . (p. ).

Sound Pressure Level (dB)

is the decibel level. For either general or acoustic data, when the sampled data is pressure (for example,

static pressure or sound pressure), the Sound Pressure Level (dB) (

) is calculated in decibel units

using

(.)

where

is the Power Spectral Density for either a particular Fourier mode or a particular

frequency band (see Equation . (p. ) and Equation . (p. )).

acoustic pressure, with a default value of   - Pa; you can revise this value, as described in

Enabling the FW-H Acoustics Model (p. ).

Sound Amplitude (dB)

is similar to the Sound Pressure Level (dB), and is a logarithmic conversion of the pressure signal

Magnitude into decibel units.The Sound Amplitude (dB) (

) is calculated for either a Fourier mode

or a frequency band using

(.)

A-Weighted, Sound Pressure Level (dB A)

is the calculated sound pressure level weighted by the A-scale function to more closely approximate

the frequency response of the human ear. A-Weighting is applied for loudness levels below  phons

( dB at  kHz) and is the most commonly used weighting function. See Figure . : A-, B-, and C-

Weighting Functions (p. ) for a graphical representation.This function is only available when the X

Axis Function is either Octave Band or /-Octave Band.

B-Weighted, Sound Pressure Level (dB B)

is the calculated sound pressure level weighted by the B-scale function. B-Weighting is applied to

loudness levels between  and  phons, though it is rarely used. See Figure . : A-, B-, and C-

C-Weighted, Sound Pressure Level (dB C)

is the calculated sound pressure level weighted by the C-scale function. C-Weighting is applied for

loudness levels above  phons and is commonly used for high-intensity sound such as traffic studies.

See Figure . : A-, B-, and C-Weighting Functions (p. ) for a graphical representation.This function

is only available when the X Axis Function is either Octave Band or /-Octave Band.

Figure . : A-, B-, and C-Weighting Functions

Further graphical customizations for the -axis are available by clicking the Axes... button. For more

information, see Modifying Axis Attributes (p. ).

..... Specifying a Function for the X Axis

There are three options for the -axis function you can choose from in order to plot or write the

detailed spectrum with all resolved Fourier modes; these three options are related to the discrete

frequencies at which the Fourier coefficients are computed. There are also two additional options

available when the Acoustics Analysis option is enabled, which allow the octave and / octave

band analysis. You can apply specific analytic functions for the -axis using the X Axis Function

Available options for the -axis functions are as follows. The definitions are provided for

,

because the corresponding definitions for the -axis functions include contributions from both ele-

ments of a complex conjugate pair  and

is always

an even number.

Frequency (Hz)

is defined as:

(.)

where

is the number of data points used in the FFT.

Strouhal Number

is always

(.)

where

is the nondimensionalized version of the frequency defined in Equation . (p. ) :

(.)

where

and

are the reference length and velocity scales specified in the Reference Values

Task Page (p. ).

Fourier Mode

is the index in Equation . (p. ) and/or Equation . (p. ), which represents the

th term in

the Fourier transform of the signal.

Octave Band (Hz)

is a range of discrete frequency bands for different octaves within the threshold of hearing.The range

of each octave band is double to that of the previous band (see Table . : Octave Band Frequencies

and Weightings (p. )).

/-Octave Band (Hz)

is a range of discrete frequency bands for different / octaves within the threshold of hearing.

Table . : Octave Band Frequencies and Weightings

dB C

dB B

dB A

Upper

Freq. (Hz)

Center

Freq. (Hz)

Lower

Freq. (Hz)

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

.

Further graphical customizations for the -axis are available by clicking Axes.... For more information,

see Modifying Axis Attributes (p. ).

..... Specifying Output Options

You can write out the FFT data directly to a file by choosing the Write FFT to File option under

Options in the Fourier Transform Dialog Box (p. ). Once the Write FFT to File option is selected,

click Write FFT to display a file selection dialog box where you can choose a file and/or a location

to hold the FFT data. If Acoustics Analysis is selected, the overall sound pressure level will be calcu-

lated in dB (based on the Reference Acoustic Pressure) and displayed in the console at this time.

Further customizations for how the FFT data is displayed are available by clicking Curves.... For more

information, see Modifying Curve Attributes (p. ).

..... Specifying a Windowing Technique

You can use the various windowing techniques described in Windowing (p. ) by selecting any of

the Window options in the Plot/Modify Input Signal Dialog Box (p. ). By default, None is selected

so that no windowing technique is applied.

..... Specifying Labels and Titles

You can assign a title for your FFT plot using the Plot Title text field. You can also assign -axis and

axis labels for your FFT plot using the Y Axis Label and X Axis Label text fields, respectively. By

default,ANSYS Fluent assigns the Y Axis Label and the X Axis Label to the particular selection of Y

Axis Function and X Axis Function.

Chapter : Reporting Alphanumeric Data

ANSYS Fluent provides tools for computing and reporting integral quantities at surfaces and boundaries.

These tools enable you to find the mass flow rate and heat transfer rate through boundaries, the forces

and moments on boundaries, and the area, integral, flow rate, average, and mass average (among

other quantities) on a surface or in a volume. In addition, you can print histograms of geometric and

solution data, set reference values for the calculation of non-dimensional coefficients, and compute

projected surface areas. You can also print or save a summary report of the models, boundary conditions,

and solver settings in the current case. These features are described in the following sections.

.. Reporting Conventions

.. Monitoring and Reporting Solution Data

.. Creating Output Parameters

.. Fluxes Through Boundaries

.. Forces on Boundaries

.. Projected Surface Area Calculations

.. Surface Integration

..Volume Integration

.. Histogram Reports

.. Discrete Phase

.. S2S Information

.. Reference Values

.. Summary Reports of Case Settings

.. System Resource Usage

Reporting tools for the discrete phase are described in Postprocessing for the Discrete Phase (p. ).

For 2D problems, ANSYS Fluent computes all integral quantities for a unit depth equivalent to  meter.

This value can be adjusted to match the specific dimension of your application only by manually revising

the Depth in the Reference Values Task Page (p. ) (see Reference Values (p. )).

Important

The default value of Depth will be equivalent to  meter, even if the units are changed for

depth in the Set Units Dialog Box (p. ) (for example, if the units for depth are changed

to cm in the Set Units Dialog Box (p. ), the value of Depth in the Reference Values Task

Page (p. ) will be

cm).

Note that inputs for DPM and fluid massflow are always assumed to correspond to a 1m deep version

of the model model and are scaled accordingly. For example, if the reference Depth is set to . m, ef-

fectively reducing the model by half, massflows used in volume integral calculations will be half of the

original massflows.

For axisymmetric problems, all integral quantities are computed for an angle of

radians.

During the course of a simulation, you may want to monitor, print, write, and/or plot solution data; this

radians.

is done using report definitions. A report definition is an object that specifies a certain quantity or set

of values to be computed at the end of a solver timestep or iteration. You can then choose to have

multiple report definitions printed to the console, written to a single file, or plotted in the same window.

You can use report definitions to monitor convergence, verify mesh independence, and record time-

histories. These report definitions can monitor the value of field variables or functions through specified

operations, such as surface, volume, force, moment, and flux integrals.

Once you create report definitions, they can be added to a report file. Report files can include multiple

report definitions of varied types. Multiple report definitions can be plotted in the same graphics window

by adding them to a single report plot. One report definition can be included in multiple report plots

and files. For additional information on report files and plots, see Report Files and Report Plots (p. ).

... Creating Report Definitions

You can create report definitions from multiple locations in Fluent, allowing you to quickly define report

definitions, regardless of where you are in your workflow. The primary method to create a report

definition is through the ribbon. For example:

Solution → Reports → Definitions → New → Surface Report → Area-Weighted Average...

Opens the Surface Report Definition dialog box.

Alternative methods for accessing this dialog box are through the tree, by right-clicking the Report Defin-

ition branch, or through the New drop-down list in the Figure . : Report Definitions Dialog Box (p. ).

Reporting Alphanumeric Data

Many of the setup steps are the same or similar when setting up the various types of report definitions.

To setup the Surface Report Definition dialog box:

. Enter a name for the report definition under Name.

. If you want the value reported on individual surfaces rather than the net results from a group of surfaces,

enable the Per Surface option.

. (optional) To have Fluent calculate a running average for the Surface Report Definition you can enter

a positive integer greater than  (the default) for Average Over.

Specifying a number greater than  means that Fluent will print, plot, and write the running average

value of the selected variable instead of the current value of the same variable.

The value reported is averaged over the last

iterations/time steps, where

is your specified Average

Over value. When the iteration/time step number is lower than

, Fluent calculates the average of the

available variable values.

Monitoring and Reporting Solution Data

. If you want the report definition written to a file or plotted, either select an existing report file or plot

from the Report Files or Report Plots lists, or create a new report file or plot by enabling Report File

and/or Report Plot in the Create group box.

. If you want the report definition available as an output parameter, enable Create Output Parameter.

. Choose the surface report definition integration method by selecting Area, Integral, Standard Deviation,

Flow Rate, Mass Flow Rate, Volume Flow Rate, Area-Weighted Average, Mass-Weighted Average,

Sum, Uniformity Index - Mass Weighted, Uniformity Index - Area Weighted, Facet Average, Facet

Minimum, Facet Maximum, Vertex Average, Vertex Minimum, Vertex Maximum, Custom Vector

Based Flux, Custom Vector Flux, or Custom Vector Weighted Average from the Report Type drop-

down list.These methods are described in Surface Integration (p. ).

. If you selected Custom Vector Based Flux, Custom Vector Flux, or Custom Vector Weighted Average

from the Report Type drop-down list, you must define the vectors in the Custom Vectors group box.

. Unless you are reporting a mass flow rate or volume flow rate, specify the variable or function to be integ-

rated in the Field Variable drop-down list. First select the desired category in the upper drop-down list.

You can then select one of the related quantities in the lower list. (See Field Function Definitions (p. )

for an explanation of the variables in the list.) If you are running a multiphase simulation you may need

to select the phase of interest (or mixture) from the Phase drop-down list (depending on the field variable

Note

In general, you can select any arbitrary field variable for each report type. However, not all

possible combinations are physically meaningful.

For multiphase flow, you should use only the Mass Flow Rate integral to compute the mass

flow rate of the mixture or for an individual phase. Do not use the Flow Rate integral of the

Volume Fraction field variable as this will result in erroneous results.

. Select the Surfaces where you want Fluent to evaluate the specified variable.

. You have the option to highlight a selected surface and have it displayed in the graphics window by en-

abling Highlight Surfaces.

. Click OK to create the report definition and close the dialog box.

Once you have created a report definition, it appears in the Figure . : Report Definitions Dialog Box (p. ).

Figure . : Report Definitions Dialog Box

You can use this dialog box to review and modify the properties of the existing report definitions.

Note

The report definitions that are automatically created for transient simulations (flow-time,

delta-time, iters-per-timestep) are not available for export or copying.

The following sections detail setup instructions that are specific to each type of report definition.

.... Surface Report Definitions

....Volume Report Definitions

.... Force and Moment Report Definitions

.... Flux Report Definition

.... DPM Report Definition

.... User Defined Report Definition

.... Expression Report Definition

You can use the Figure . : Surface Report Definition Dialog Box (p. ) to create surface report

definitions. There are many different types of surface-based report definitions that you can create,

Integral

Standard Deviation

Flow Rate

Mass Flow Rate (non-field based)

Volume Flow Rate (non-field based)

Area-Weighted Average

Mass-Weighted Average

Sum

Uniformity Index — Mass Weighted

Uniformity Index — Area Weighted

Facet Average

Facet Minimum

Facet Maximum

Custom Vector Based Flux (custom-vector based)

Sum

Custom Vector Flux (custom-vector based, non-field based)

Custom Vector Weighted Average (custom-vector based)

To plot or write the surface report definition data you must use a Report File or Report Plot. If a

surface report definition is already included in a report file/plot, then that report file/plot will be

highlighted. If you de-select a report file/plot that had included the current report definition and click

OK, the report definition will be removed from that report file/plot. For additional information on

report files and plots, see Report Files and Report Plots (p. ).

Solution → Reports → Definitions → New → Surface Report

Figure . : Surface Report Definition Dialog Box

The procedure for creating surface report definitions is covered in Creating Report Definitions (p. ).

You can use the Figure . : Volume Report Definition Dialog Box (p. ) to create volume report

definitions. There are many different types of volume reports that you can create, including:

Volume (non-field based)

Sum

Sum*

(only axi-symmetric)

Max

Min

Volume Integral

Volume Average

Mass Integral

Mass Average

Mass (non-field based)

Solution → Reports → Definitions → New → Volume Report

Figure . : Volume Report Definition Dialog Box

The common steps for creating a volume report definition are covered in Creating Report Defini-

tions (p. ), and the volume report definition-specific steps are as follows:

. If you want the value reported on individual wall zones rather than the net results from a group of wall

zones, enable the Per Zone option.

. Choose the integration method for the volume report definition by selecting Volume, Sum, Sum*2Pi

(2D axisymmetric cases only), Max, Min, Volume Integral, Volume-Average, Mass Integral, Mass-Av-

erage, or Mass in the Report Type drop-down list.These methods are described in Volume Integra-

tion (p. ).

. Specify the variable or function to be integrated in the Field Variable drop-down list. First select the

desired category in the upper drop-down list.You can then select one of the related quantities in the

lower list. (See Field Function Definitions (p. ) for an explanation of the variables in the list.)

. Select the Cell Zones where you want Fluent to evaluate the specified variable.

Monitoring force coefficients can be useful when you are calculating external aerodynamics, for ex-

ample, and are especially interested in the lift coefficient. By monitoring these values you may also

be able to stop the calculation early and reduce the processing time, as sometimes the force and

moment coefficients converge before the residuals have decreased three orders of magnitude. (In

such an instance, you should be sure to check the mass flow rate and heat transfer rate as well, to

ensure that the mass and energy are being suitably conserved. This is accomplished using either the

Figure . : Drag Report Definition Dialog Box (p. ), the Figure . : Lift Report Definition Dialog

Box (p. ), the Figure . : Moment Report Definition Dialog Box (p. ), or the Figure . : Force

Report Definition Dialog Box (p. )).

To begin setting up force or moment report definitions, first enter appropriate values in the Reference

Values task page, as described in Reference Values (p. ). The relevant values include the following:

The force coefficients use the reference area, density, and velocity.

The moment coefficients use the reference area, density, velocity and length.

For information about how these coefficients are calculated, see Computing Forces, Moments, and the

Center of Pressure in the Fluent Theory Guide.

Tip

You can have Fluent report unscaled force values by selecting Drag Force or Lift Force

in the Report Output Type group box of the Drag Report Definition or Lift Report

Definition dialog boxes, respectively.

Next, open the appropriate dialog box through the Solution tab of the ribbon.

Solution → Reports → Definitions → New → Force Report

Select either Drag..., Lift..., Moment..., or Force... to open the Figure . : Drag Report Definition

Dialog Box (p. ), Figure . : Lift Report Definition Dialog Box (p. ), Figure . : Moment Report

Definition Dialog Box (p. ), and Figure . : Force Report Definition Dialog Box (p. ). Note that

you can only access one of these report definition dialog boxes at a time, though multiple report

definitions of the same type can be used during the simulation.

Figure . : Force Report Definition Dialog Box

Figure . : Drag Report Definition Dialog Box

Figure . : Lift Report Definition Dialog Box

Figure . : Moment Report Definition Dialog Box

The common steps for creating a force or moment report definition are covered in Creating Report

Definitions (p. ), and the force/moment report definition-specific steps are as follows:

. If you want to report the force or moment coefficient data from individual wall zones rather than the

net results from a group of wall zones, enable the Per Zone option.

. Depending on the coefficient that will be monitored, perform one of the following steps:

In the Drag Report Definition, Lift Report Definition or Force Report Definition dialog box, enter

the X, Y, and Z components of the Force Vector along which the forces will be computed. By default,

the Force Vector for the drag coefficient is a unit vector in the  direction, whereas for the lift coefficient

it is a unit vector in the  direction.

In the Moment Report Definition dialog box, enter the Cartesian coordinates (X, Y, and Z) of the

Moment Center, about which moments will be computed.The default Moment Center is (, , ).

You also need to enter the X, Y, and Z components for the Moment Axis, along which the moment

coefficient will be calculated. By default, the Moment Axis is defined as a unit vector in the  direction.

. Select the appropriate wall zone(s) for computation of the coefficient(s).

. You have the option to highlight a selected boundary zone and have it displayed in the graphics window

by enabling Highlight Zone.

. Click OK to save the report definition settings.

. If you need to revise the settings of a particular report definition after they have been saved, double-

click the report definition in the tree.

You can use the Figure . : Flux Report Definition Dialog Box (p. ) to create flux report definitions.

There are many different types of flux-based report definitions that you can create, including:

Total Heat Transfer Rate

Total Sensible Heat Transfer Rate

Radiation Heat Transfer Rate

Film Mass Flow Rate

Film Heat Transfer Rate

Solution → Reports → Definitions → New → Flux Report

Figure . : Flux Report Definition Dialog Box

Figure . : DPM Source Report Definition Dialog Box

The common steps for creating a flux report definition are covered in Creating Report Defini-

tions (p. ), and the flux report definition-specific steps are as follows:

. Select or confirm the type of flux report.

. Select the appropriate boundaries for the flux calculations.

For additional information on the available options for DPM source report definitions, see DPM Source

Report Definition (p. ) in the reference guide.

You can use the DPM Report Definition dialog box to create DPM report definitions. The following

types of DPM reports are available:

Injected Mass (unsteady particle tracking only): Reports the total DPM mass injected into the domain.

Mass in Domain (unsteady particle tracking only): Reports the total DPM mass present in the domain.

Mass in Fluid (unsteady particle tracking only): Reports all DPM mass currently residing as free-stream

particles in the domain.This option is available only with the wall-film DPM boundary condition.

Mass in Film (unsteady particle tracking only): Reports all DPM mass currently residing in Lagrangian wall-

film.This option is available only with the wall-film DPM boundary condition.

Escaped Mass: Reports the DPM mass that has left the domain through a certain boundary or boundaries.

Evaporated Mass: Reports the total evaporated DPM mass for the selected injection(s).The quantity ac-

counts for fully evaporated particles as well as all mass that has evaporated from any other particles. For

unsteady tracking, this includes particles that are still present in the domain.

Penetration Length (unsteady particle tracking only): Reports the total penetration length in meters.

Solution → Reports → Definitions → New → DPM Report

Figure . : DPM Report Definition Dialog Box

The common steps for creating a DPM report definition are covered in Creating Report Defini-

tions (p. ), and the DPM report definition-specific steps are as follows:

. Select or confirm the type of DPM report.

. For the Escaped Mass report, if you want to have the escaped mass calculated per injection, enable the

text command report/dpm-zone-summaries-per-injection.

The Injections selection list will then appear in the DPM Report Definition dialog box.

. From the Injections list, select the appropriate injections for the DPM report.

Note

For the Escaped Mass report, this step is relevant only if you have enabled the calcu-

lation of the escaped mass per injection.

. For the Escaped Mass report, select the boundary(s) where the injected particles exit the domain from

the Boundaries selection list.

. For the Penetration Length report, you can specify the Particles Mass Fraction.You can also enable

User-Specified Origin and Direction to specify those coordinates.

. For unsteady particle tracking, you can select Show Mass Flow/Change Rate (default) for the Injected

Mass, Mass in Domain, Mass in Fluid, Mass in Film, Escaped Mass, and Evaporated Mass reports if

you want to create a report for the mass flow rate rather than the total mass.

Important

For unsteady particle tracking, if you want to select one or more injection(s) for any Escaped

Mass report, you must enable the report/dpm-zone-summaries-per-injection

text command before the first particles are injected; otherwise, some of the reported values

may become inconsistent.

For additional information on the available options, see the DPM Report Definition Dialog Box (p. )

in the reference guide.

User defined report definitions allow you to create functions that return values that can be plotted,

printed, written, or used in other expressions. User defined report definitions can also be used in the

Convergence Conditions (Convergence Conditions (p. )).

Creating a user defined report definition is a two step process:

. Create a user defined report definition function.

. Hook the user defined report definition function to the user defined report definition.

..... User Defined Report Definition Function

User defined report definition functions are defined with the DEFINE_REPORT_DEFINITION_FN

macro, which takes the function name as the argument. The function must return a real value. Once

written, it should be compiled and loaded the same way as other user-defined functions, see Inter-

preting and Compiling UDFs in the Fluent Customization Manual for more information.

The function body should be constructed similarly to any C function that returns a real value. Any

valid C code can be included in the function body.

DEFINE_REPORT_DEFINITION_FN can use all of the APIs available for other user-defined functions,

Last evaluated values of all report definitions.

Current values of all input parameters that have been set to be used inside user-defined functions.

See DEFINE_REPORT_DEFINITION_FN in the Fluent Customization Manual for information on

writing user defined report definition functions.

..... User Defined Report Definition Function Hooking

With the user defined report definition function written, you must hook this function to the user

defined report definition.

The common steps for creating a user defined report definition are covered in Creating Report

Definitions (p. ), and the user defined report definition-specific steps are as follows:

. Open the User Defined Report definition dialog box.

New → User Defined

Figure . : User Defined Report Definition Dialog Box

. Select your function from the Function drop-down list.

You can create expressions from report definitions, allowing you to combine report definitions with

mathematical operators to create a new report definition that can be written or plotted. For example,

you can create a pressure-drop report for the difference in area-weighted pressures between an inlet

and an outlet. You can also use an expression report definition to modify a single report definition

with expression functions such as a mathematical function or reduction operation.

Solution → Reports → Definitions → New → Expression

Figure . : Expression Report Definition Dialog Box

The common steps for creating an expression report definition are covered in Creating Report

Definitions (p. ), and the expression report definition-specific steps are as follows:

. Create the Report Definition(s) that you will use to create an Expression.

. Use the drop-downs to the right of the Definition box to select the report definition(s) and other variables

and functions, as required to define your desired expression report definition. You can also directly enter

the expression into the Definition box—the drop-downs are available to make the process easier.

Note

definition or a cell register, automatic suggestions are disabled and you must provide

the display name of that object.

. Click OK to create the expression report definition.

Refer to Fluent Expressions Language (p. ) for additional information on creating expressions.

... Report Files and Report Plots

Report Files and Report Plots are collections of report definitions that are written to a single file (report

file) or plotted to a graphics window (report plot) at specified intervals. In steady-state cases, report

files are evaluated at the specified iteration, whereas in transient cases you have the option to specify

the evaluation frequency based on iterations or timesteps.

Report definitions in the same Report Plot must have the same units.

Report Files Format:

"<report-file-name>"

"Iteration"|"Timestep" "<first-report-def-name> etc.."

("Iteration"|"Timestep" "<report-def--name>" "<report-def--name>"...)

<Iteration/Timestep> <report-def--value> <report-def--value>...

Report definitions included in a report plot are plotted in the specified window at the specified fre-

quency. It is possible to plot the same report in multiple windows. Both report plots and report files

provide the option to print to the console. You can deactivate the writing and plotting of individual

report files and plots for a particular calculation; deactivated report files and plots can be re-activated

at a later time.

.... Creating Report Files

In order to create a report file you must have first created a report definition.

Solution → Monitors → Report Files

New...

Figure . : New Report File Dialog Box

.

Provide a name for how you want this report file to appear in the Fluent tree.

You have the option to deactivate the writing of this report file by de-selecting the Active check box

to the right of the Name.

.

Select one or more report definitions from Available Report Definitions and click Add>>, to specify

the reports you want written to the same file.

.

Provide an appropriate name in the File Name text box.The Full File Name that appears below the

File Name field is created with a run index and iteration/time step index, appended to the base name.

.

Specify the frequency at which you want the report definitions written to the file.

Note

In a transient simulation, If you specify an Average Over value in a report definition,

you must set Get Data Every to time-step or flow-time. If you set Get Data Every

to iteration, Fluent will use the instantaneous value of the report definition.

.

Click OK to save the new report file.

You have the option to view—and edit —properties of report files that you created previously by

.

selecting Edit... when you right-click Report Files in the tree, which opens the Figure . : Report

File Definitions Dialog Box (p. ).

Note that you can also right-click an individual report definition to modify it directly.

Figure . : Report File Definitions Dialog Box

Selecting a report file to modify opens the Figure . : Edit Report File Dialog Box (p. ).

Figure . : Edit Report File Dialog Box

.... Creating Report Plots

In order to create a report plot you must have first created a report definition.

Solution → Monitors → Report Plots

New...

Figure . : New Report Plot Dialog Box

.

Provide a name for how you want this report plot to appear in the Fluent tree.

You have the option to deactivate the plotting of this report plot by de-selecting the Active check

box to the right of the Name.

.

the reports you want plotted in the same window.

.

Provide an appropriate names in the Plot Title and Y-Axis Label group boxes.

.

Specify the frequency at which you want the report definitions plotted to the specified window.

Note

.

Click OK to save the new report plot.

You have the option to edit report plots that you created previously by selecting Edit... when you

.

right-click Report Plots in the tree, which opens the Figure . : Report Plot Definitions Dialog

Box (p. ).

Once you begin iterating, Fluent displays report plots in the graphics window. If you close the

graphics window containing a plot, you can redisplay it by right-clicking the report plot in the Outline

View tree and selecting Plot.

Figure . : Report Plot Definitions Dialog Box

Selecting a report plot to modify opens the Figure . : Edit Report Plot Dialog Box (p. ).

Figure . : Edit Report Plot Dialog Box

You can create output parameters, which allow you to compare reporting values for different cases, or

include reporting values in the function minimized by the mesh morpher/optimizer. These are single

values generated by a variety of reports:

Fluxes (Fluxes Through Boundaries (p. ))

Forces (Forces on Boundaries (p. ))

Surface integrals (Generating a Surface Integral Report (p. ))

Volume integrals (Generating a Volume Integral Report (p. ))

Surface report definitions (Surface Report Definitions (p. ))

Volume report definitions (Volume Report Definitions (p. ))

Drag report definitions (Force and Moment Report Definitions (p. ))

Lift report definitions(Force and Moment Report Definitions (p. ))

Moment report definitions(Force and Moment Report Definitions (p. ))

Force report definitions(Force and Moment Report Definitions (p. ))

Creating Output Parameters

User Defined report definitions(User Defined Report Definition (p. ))

Expression report definitions (Expression Report Definition (p. ))

Click Parameters... in the User Defined ribbon tab (Field Functions group box) to open the Parameters

Dialog Box (p. ), where a list of any previously created input parameters is available.

User Defined → Field Functions → Parameters...

The list of Input Parameters is populated after performing the steps outlined in Defining and Viewing

Parameters (p. ). The output parameters that you create will be listed under Output Parameters.

You can define the output parameters using the reporting dialog boxes, as described in Creating Report

Definitions (p. ). The reporting dialog boxes are accessible Definitions drop-down list in the Solution

ribbon tab (Reports group box). Clicking the Create drop-down list under Output Parameters in the

Parameters dialog box allows you to select From Report Definitions..., which opens the Figure . : Re-

port Definitions Dialog Box (p. ). From there you can create any type of report definition.

Once you have saved your output parameters, you can modify their definitions by selecting the para-

meter in the Output Parameters list and clicking Edit.... This will open the report dialog box where

you can make your changes.

In addition, you can select any of the following commands under the More drop-down list:

Delete

Rename

allows you to rename the selected output parameter.

reports values to the console window. If you select multiple output parameters, then the output includes

values from multiple output parameters.

Write...

This section contains information about generating a flux report. For more background information,

see Fluxes Through Boundaries in the Theory Guide .

... Generating a Flux Report

... Flux Reporting for Reacting Flows

... Flux Reporting with Particles

... Flux Reporting with Multiphase

... Flux Reporting with Other Volumetric Sources

To obtain a report of mass flow rate, total heat transfer rate, total sensible heat transfer rate, or radiation

heat transfer rate on selected boundary zones, use the Flux Reports Dialog Box (p. ) (Figure . : The

Flux Reports Dialog Box (p. )).

Edit...

Figure . : The Flux Reports Dialog Box

Fluxes Through Boundaries

. Specify which flux computation you are interested in by selecting one of the following under Options:

The net flux from volumetric radiation sources is reported in the Net Radiation Source field.

Film Mass Flow Rate (available as an option only when the Eulerian Wall Film model is enabled—see

Modeling Eulerian Wall Films (p. ))

Film Heat Transfer Rate (available as an option only when the Eulerian Wall Film model is enabled—see

. In the Boundaries list, choose the boundary zone(s) on which you want to report fluxes.

You can use Filter Text entry box to filter the Boundaries list to show only the boundary zones

that match the pattern you enter. For additional information on using the Filter Text entry box,

see Filter Text Entry Boxes (p. ).

. To create an output parameter for the reported value, click Save Output Parameter....The Save Output

Parameter Dialog Box (p. ) (Figure . :The Save Output Parameter Dialog Box (p. )) will open

where you will specify the name of the newly created output parameter, or overwrite an existing output

parameter of the same type. ANSYS Fluent automatically creates generic default names for new input and

output parameters (for example, parameter-, parameter-, and so on).

Figure . : The Save Output Parameter Dialog Box

After the output parameter is created, it is listed in the Parameters Dialog Box (p. ), accessed via

the Parameters... button in the Reports Task Page (p. ). You can create any number of output

parameters of this report type.

Note

If you create an output parameter from a flux report and save the case and data (write),

an equivalent report definition will be created when you read in the case file.

. Click the Compute button to display the results of the selected flux computation for each selected

The Net Results field shows the summation of the individual zone flux results. If you specified the

mass source terms in the Fluid dialog box, the integral mass flow rate value from the user-specified

sources is reported in the User Source field and is added to the Net Results. Similarly, if you spe-

cified the energy source terms in the Fluid dialog box, the integral total heat transfer rate value

from the user-specified sources is reported in the User Source field and is added to the net heat

balance results reported in Net Results.

Important

Additional steps must be taken prior to generating a flux report for an interior boundary zone

that has the same fluid defined on either side. In such a case, the area vectors of the cell faces

associated with the zone may have been automatically defined in an inconsistent manner when

the mesh file was read into the solver. Since the flux for each individual cell face is calculated

with respect to its area vector, such an inconsistency leads to inaccurate results when the face

fluxes are summed to calculate the total flux of the boundary zone.

To ensure accurate flux results for such an interior zone, you must orient the area vectors by

changing the definition of the zone Type to wall.You should then change the Type back to

interior and proceed to generate the flux report.

Mass Flow Rate is calculated through the simulation domain or the specified zones. However,

if you specify only the interior zone(s), the net mass flow rate may show as , because these in-

ternal boundaries are skipped when ANSYS Fluent computes the net influx and outflux.

Note that the fluxes are reported exactly as computed by the solver. Therefore, they are inherently

more accurate than those computed with the Flow Rate option in the Surface Integrals Dialog

Box (p. ) (described in Surface Integration (p. )).

To report heat transfer for reacting flows, one of models in the Species Model Dialog Box (p. ) must

be enabled for the Total Sensible Heat Transfer Rate option to appear in the Flux Reports Dialog

Box (p. ). For reacting flows, ANSYS Fluent produces two kinds of reports that use a different treatment

at the flow boundaries:

Total Heat Transfer Rate reports the total enthalpy flux, which consists of the thermal enthalpy, plus the

species formation enthalpy when Volumetric Reactions are enabled.The heat rate based on this definition

is a conserved quantity in reacting flows. See Heat Transfer Theory in the Theory Guide  for details.

Total Sensible Heat Transfer Rate reports the total energy flux as defined in Equation . in the Theory

Guide . Note that in reacting flows, this is not a conserved quantity and the addition or removal of heat

due to the chemical reactions (Equation . in the Theory Guide ) is reported separately in the Heat of

Reaction Source field, as shown in Figure . :The Flux Reports Dialog Box (p. ). If you have more than

one reaction defined in your case, the Heat of Reaction Source reported is the sum of the heat for all re-

actions. For exothermic reactions the Heat of Reaction Source is reported as a positive quantity, while for

endothermic reactions it will be a negative quantity.

Important

Note that both the Total Heat Transfer Rate and Total Sensible Heat Transfer Rate options

report a Net Result, which may be used as an indication of the energy balance for the case.

In general, and if heat sources other than the heat of reaction and DPM are not included

in your problem, the Net Result reported in both the Total Heat Transfer Rate and Total

Sensible Heat Transfer Rate options should be a small number for a converged calculation.

However, if a reacting case is not well converged for both energy and species transport

equations, the Net Result reported in the Total Heat Transfer Rate and Total Sensible

Heat Transfer Rate options may differ. In that case, you may consider iterating further to

achieve a fully converged solution. In addition, refer to the sections that follow for special

considerations when including particles, multiphase models, or other volumetric energy

sources.

Important

Note that for the non-premixed and partially premixed models the Heat of Reaction Source

is calculated as the difference of the net Total Heat Transfer Rate and the net Total

Sensible Heat Transfer Rate. The Heat of Reaction field function is not available for the

non-premixed and partially-premixed models.

If you are using the discrete phase model (DPM), the contributions from the particle injections are re-

ported separately and are included in the net mass and heat balance results. Consequently, the Mass

Flow Rate report includes the DPM Mass Source, the Total Heat Transfer Rate report includes the

DPM Enthalpy Source, and the Total Sensible Heat Transfer Rate includes the DPM Sensible En-

thalpy Source (Figure . : The Flux Reports Dialog Box with DPM (p. )).

Figure . : The Flux Reports Dialog Box with DPM

For P1 or discrete ordinates (DO) radiation simulations, if Particle Radiation Interaction is selected

in the Physical Models tab of the Discrete Phase Model dialog box, the Radiation Heat Transfer

Rate reports the difference between the radiation emitted and the radiation absorbed on the surface

of the particles in the DPM Radiation Source field.

Important

In the case of reacting flows with the DPM model, the Heat of Reaction Source entry reports

the heat of all homogeneous reactions in the continuous phase, while the heat released or

consumed due to particle reactions (e.g, char combustion) is reported in the DPM Sensible

Enthalpy Source field.

If you are using any of the multiphase models, the mass or heat rates can be reported separately for

each phase and for the mixture phase. If you specified the mass source terms in the cell zone conditions

dialog box for a specific phase, then the integral mass flow rate value from the user-specified sources

is reported for the relevant phase in the User Source field and is added to the net mass balance results

reported in Net Results. Similarly, if you specified the energy source terms in the cell zone conditions

dialog box for a specific phase, the integral total heat transfer rate value from the user-specified sources

is reported for the relevant phase in the User Source field and is added to the net heat balance results

reported in Net Results. For the Eulerian multiphase model, in addition to reporting for the phases,

the user source flux is also reported for the mixture.

Note that if your multiphase model includes mass or heat transfer processes between phases, the mass

and heat transferred across the phases will be reported as an imbalance in the report of each phase.

In order to check the overall balances for the multiphase cases you should select the mixture phase

for your report. In that case, the report will include the sum of the fluxes and sources for all phases

included in your model.

Finally, if you are solving a multiphase problem that includes chemical reactions, you should be aware

of the following conventions when you are requesting a Total Sensible Heat Transfer Rate report:

If you select one of the phases with gas phase chemical reactions, the Heat of Reaction Source will only

include contributions from reactions in the particular phase.

When you report the Total Sensible Heat Transfer Rate for the mixture phase, the Heat of Reaction

Source entry will report the sum of the heat of reaction of all gas phase reactions in all phases plus the

heat of any heterogeneous reactions that take place.

The reported mass and heat balances address the flow that enters or leaves the domain through

boundaries and the contributions from DPM sources and user-defined sources; they do not include

the contributions from other volumetric sources, such as the heat exchanged in the Heat Exchanger

Model. For this reason, a mass or heat imbalance may be reported. In that case, and in a converged

calculation, the reported imbalance will be equal to that volumetric source.

For a Radiation Heat Transfer Rate flux report, the Net Radiation Source field provides the net flux

from volumetric radiation sources and is computed as the difference between the emitted and absorbed

volumetric radiation sources.

For wall zones that you select, you can compute and report the forces along a specified vector, the

moments about a specified center and along a specified axis, and the coordinates of the center of

pressure. This feature is useful for reporting, for instance, aerodynamic quantities such as lift, drag, and

moment coefficients, as well as the center of pressure for an airfoil.

For additional information about forces, moments, and the center of pressure, see Computing Forces,

Moments, and the Center of Pressure in the Theory Guide .

... Generating a Force, Moment, or Center of Pressure Report

To obtain a report (for selected wall zones) of forces along a specified vector, moments about a specified

center and along a specified axis, or the center of pressure, use the Force Reports Dialog Box (p. )

(Figure . : The Force Reports Dialog Box (p. )).

Edit...

Figure . : The Force Reports Dialog Box

. Specify the type of report in which you are interested by selecting Forces, Moments, or Center of Pressure

from the Options list.

. Define the settings associated with report you are generating:

a.

For a force report, enter the X, Y, and Z components of the Force Vector along which the forces will

be computed.

Important

If

(the -component of the force) is zero, then either the Y or Z coordinate can

be fixed. If

is zero, then either the X or Z coordinate can be fixed. If

is zero,

then either the X or Y coordinate can be fixed.

b. For a moment report, enter the X, Y, and Z coordinates of the Moment Center about which the mo-

ments will be computed, as well as the X, Y, and Z components of the Moment Axis along which the

moments will be computed.

c.

For a center of pressure report, define the line (for 2D geometries) or plane (for 3D geometries) on

which you want to calculate the center of pressure.The line or plane must have one of its coordinate

values fixed (for example, a line defined as

). Select the axis (X, Y, or Z) in the Coordinate group

box, and then enter the fixed Value. See the example at the end of this section for further details.

. In the Wall Zones list, select the wall zone(s) for which you want a report of the forces, moments, or

pressure center.

Forces on Boundaries

After the output parameter is created, it is listed in the Parameters Dialog Box (p. ). You can

create any number of output parameters of this report type.

Note

If you create an output parameter from a force, moment, or center of pressure report

and save the case and data (write), an equivalent report definition will be created when

you read in the case file.

. Click the Print button if you want the results displayed in the console window, or click Write... to save it

to a file.

If you selected Forces under Options, the pressure force, viscous force (if appropriate), total forces,

pressure coefficient, viscous coefficient, and total coefficients for each selected wall zone will be

displayed or saved.

If you selected Moments, the pressure moments, viscous moments (if appropriate), total moments,

pressure coefficient, viscous coefficient and total coefficients for the wall zones about the specified

center will be displayed or saved. Additionally, the moments and coefficients in the direction of

the specified axis will be displayed or saved. The report will include the values for the individual

wall zones, as well as the net values for all of the wall zones combined. See Computing Forces,

Moments, and the Center of Pressure in the Theory Guide  for details about computing forces

and moments.

If you selected Center of Pressure, then ANSYS Fluent displays or saves the coordinates about

which the moment is zero.

Important

You cannot save your output parameter if Center of Pressure is selected; Center of

Pressure is not available as an output parameter since it is a set of coordinates.

Important

Note that the reported force and moment coefficients are a function of the values entered

in the Reference Values task page (as described in Computing Forces, Moments, and the

Center of Pressure in the Theory Guide ). Therefore, appropriate values must be entered

in the Reference Values task page to get meaningful results.

To demonstrate how you would generate and interpret the center of pressure report, consider an

airfoil of chord length  m (shown in Figure . : An Airfoil with its Computed Center of Pres-

sure (p. )).

Figure . : An Airfoil with its Computed Center of Pressure

Open the Force Reports dialog box and perform the steps that follow.

Edit...

Figure . : The Force Reports Dialog Box for a Center of Pressure Report

. Select Center of Pressure from the Options list.

. Define the line on which the center of pressure will be calculated. In this case, the Y coordinate for the

line has a fixed Value of .

. Select the Wall Zones that are relevant for the computation.

. Click Print to have the coordinates of the center of pressure displayed in the console window.

The report generated will be in the following form:

Pressure Center Coordinates (in m):

X = .

Y =

You can use the Projected Surface Areas Dialog Box (p. ) (Figure . : The Projected Surface Areas

Dialog Box (p. )) to compute an estimated area of the projection of selected surfaces along the ,

,

or  axis (that is, onto the

,

, or

plane).

Edit...

Figure . : The Projected Surface Areas Dialog Box

The steps for calculating the projected area are as follows:

. Select the Projection Direction (X, Y, or Z).

. Choose the surface(s) for which the projected area is to be calculated in the Surfaces list.

. Set the Min Feature Size to the length of the smallest feature in the geometry that you want to resolve

in the area calculation. (You can just use the default value to start with, if you are not sure of the size of

the smallest geometrical feature.)

. Click Compute.The area will be displayed in the Area box and in the console window.

. To improve the accuracy of the area calculation, reduce the Min Feature Size by half and recompute the

area. Repeat this step until the computed Area stops changing (or you reach memory capacity).

This feature is available only for 3D domains.

This section describes how to compute surface integrals. For mathematical definitions of the various

integral types, refer to Computing Surface Integrals in the Theory Guide .

... Generating a Surface Integral Report

To obtain a report for selected surfaces of the area, custom vector-based flux, custom vector flux,

custom vector-weighted average, mass flow rate, or volume flow rate, or the integral, flow rate,

standard deviation, sum, facet maximum, facet minimum, uniformity index (weighted by mass or area),

vertex maximum, vertex minimum, or mass-, area-, facet-, or vertex-averaged quantity of a specified

field variable, use the Surface Integrals Dialog Box (p. ) (Figure . : The Surface Integrals Dialog

Box (p. )).

Edit...

Surface Integration

Figure . : The Surface Integrals Dialog Box

. Specify which type of report you are interested in by selecting Area, Area-Weighted Average, Custom

Vector Based Flux, Custom Vector Flux, Custom Vector Weighted Average, Facet Average, Facet

Minimum, Facet Maximum, Flow Rate, Integral, Mass Flow Rate, Mass-Weighted Average, Standard

Deviation, Sum, Uniformity Index - Mass Weighted, Uniformity Index - Area Weighted, Vertex Average,

Vertex Minimum, Vertex Maximum, or Volume Flow Rate in the Report Type drop-down list.

from the Report Type drop-down list, you must define vectors in the Custom Vectors group box.

. If you are performing a multiphase simulation, you may need to select the phase of interest from the

Phase drop-down list depending on the selected Report Type.

. If you are generating a report of area, mass flow rate, or volume flow rate, skip to the next step. Otherwise,

use the Field Variable drop-down lists to select the field variable to be used in the surface integrations.

First, select the desired category in the upper drop-down list.You can then select a related quantity from

the lower list. (See Field Function Definitions (p. ) for an explanation of the variables in the list.)

. In the Surfaces list, choose the surface(s) on which to perform the surface integration.

Note

If you create an output parameter from a surface integral report and save the case and

data (write), an equivalent report definition will be created when you read in the case

file.

. Click the Compute button.The computed results are printed in the numeric result field and also in the

ANSYS Fluent console.

The Net value reported in the ANSYS Fluent console corresponds to the specified calculation performed

over the list of selected surfaces.

. To save the computed results to a file, click the Write... button and specify the filename in the resulting

Mass averaging “weights” toward regions of higher velocity (that is, regions where more mass crosses the

surface).

Flow rates reported using the Surface Integrals Dialog Box (p. ) are not as accurate as those reported

with the Flux Reports Dialog Box (p. ) (described in Fluxes Through Boundaries (p. )).

The facet and vertex average options are recommended for zero-area surfaces.

The uniformity index represents how a specified field variable varies over a surface, where a value of  in-

dicates the highest uniformity.The uniformity index can be weighted by area or mass: the area-weighted

uniformity index captures the variation of the quantity (for example, the species concentration), whereas

the mass-weighted uniformity index captures the variation of the flux (for example, the species flux). See

Computing Surface Integrals in the Theory Guide  for the equations used to calculate the uniformity index.

This section describes how to compute volume integrals. For mathematical definitions of the various

integral types, refer to Computing Volume Integrals in the Theory Guide .

... Generating a Volume Integral Report

To obtain a report (of quantities such as the volume, sum, minimum, maximum, volume integral,

volume-weighted average, mass-weighted integral, or mass-weighted average) for selected cell zones

for a specified field variable, use the Volume Integrals Dialog Box (p. ) (Figure . : The Volume

Integrals Dialog Box (p. )).

Volume Integration

Results → Reports → Volume Integrals

Edit...

Figure . : The Volume Integrals Dialog Box

. Specify which type of report you are interested in by selecting Volume, Sum, Sum*2Pi (only available

for 2D Axisymmetric cases), Maximum, Minimum, Volume Integral, Volume-Average, Mass, Mass In-

tegral, or Mass-Average under Report Type.

. If you are generating a report of Volume or Mass, skip to the next step. Otherwise, use the Field Variable

drop-down lists to select the field variable to be used in the integral, sum, or averaged volume integrations.

. If you are performing a multiphase simulation, select the phase of interest (or mixture) from the Phase

. In the Cell Zones list, choose the zones on which to compute the volume, sum, max, min, volume integral,

volume-weighted average, mass integral, or mass-averaged quantity.

Note

If you create an output parameter from a volume integral report and save the case and

file.

over the list of selected cell zones.

In ANSYS Fluent, you can print geometric and solution data in the console (text) window in histogram

format or plot a histogram in the graphics window. Graphical display of histograms and the procedures

for defining a histogram are discussed in Histograms (p. ).

The number of cells, the range of the selected variable or function, and the percentage of the total

number of cells in the interval will be reported, as in the example below:

cells below . ( %)

cells between . and . (. %)

cells between . and . ( %)

cells between . and . (.

cells above . ( %)

To generate such a printed histogram, use the Histogram Dialog Box (p. ).

Edit...

Follow the instructions in Histograms (p. ) for generating histogram plots, but click Print instead of

Plot to create the report.

ANSYS Fluent allows you to write particle states (position, velocity, diameter, temperature, and mass

flow rate) to files at various boundaries and planes (lines in 2D) using the Sample Trajectories Dialog

Box (p. ) (Figure . : The Sample Trajectories Dialog Box (p. )). Information about discrete phase

reporting is discussed in detail in Sampling of Trajectories (p. ), Histogram Reporting of Samples (p. ),

and Summary Reporting of Current Particles (p. ).

ANSYS Fluent allows you to view the values of the view factor and radiation emitted from one zone to

another. You will use the S2S Information Dialog Box (p. ) (Figure . : The S2S Information Dialog

Box (p. )) to generate a report of these values. For details on reporting S2S information, refer to Re-

porting Radiation in the S2S Model (p. ).

You can control the reference values that are used in the computation of derived physical quantities

and non-dimensional coefficients. These reference values are used only for postprocessing.

Some examples of the use of reference values include the following:

Force coefficients use the reference area, density, and velocity. In addition, the pressure force calculation

uses the reference pressure.

Moment coefficients use the reference length, area, density and velocity. In addition, the pressure force

calculation uses the reference pressure.

Reynolds number uses the reference length, density, and viscosity.

Pressure and total pressure coefficients use the reference pressure, density, and velocity.

Entropy uses the reference density, pressure, and temperature.

Skin friction coefficient uses the reference density and velocity.

Heat transfer coefficient uses the reference temperature.

Turbomachinery efficiency calculations use the ratio of specific heats.

... Setting Reference Values

... Setting the Reference Zone

To set the reference quantities used for computing normalized flow-field variables, use the Reference

Values Task Page (p. ) (Figure . : The Reference Values Task Page (p. )).

Setup →

Reference Values

Figure . : The Reference Values Task Page

You can specify the reference values manually or compute them based on values of physical quantities

at a selected boundary zone. The reference values to be set are Area, Density, Enthalpy, Length,

Pressure, Temperature, Velocity, dynamic Viscosity, and Ratio Of Specific Heats.

For 2D problems, an additional quantity, Depth, can also be defined. This quantity will be used for

reporting fluxes and forces, as well as relevant variables computed using the Surface Integrals Dialog

Box (p. ) and the Volume Integrals Dialog Box (p. ) (for example, Area, Flow Rate, Mass Flow

Rate, Volume, and so on). You should verify that the value and units of Depth corresponds to the

depth dimension of your application prior to reporting any of the variables above.

Important

The units for Depth are set independently from the units for Length in the Set Units Dialog

Box (p. ).

If you want to compute reference values from the conditions set on a particular boundary zone, select

the zone in the Compute From drop-down list. Note, however, that depending on the boundary

condition used, only some of the reference values may be set. For example, the reference length and

area will not be set by computing the reference values from a boundary condition; you will need to

set these manually.

To set the values manually, simply enter the value for each under the Reference Values heading.

If you are solving a flow involving multiple reference frames or sliding meshes, you can plot velocities

and other related quantities relative to the motion of a specified “reference zone”. Choose the desired

zone in the Reference Zone drop-down list. Changing the reference zone allows you to plot velocities

(and total pressure, temperature, and so on) relative to the motion of different zones. See Modeling

Flows with Moving Reference Frames (p. ) for details about postprocessing of relative quantities.

You may sometimes find it useful to get a report of the current settings in your case. In ANSYS Fluent,

you can list the settings for physical models, boundary conditions, material properties, and solver controls.

This report allows you to get an overview of your current problem definition quickly, instead of having

to check the settings in each dialog box.

... Generating a Summary Report

To generate a summary report you will use the Input Summary Dialog Box (p. ) (Figure . : The

Input Summary Dialog Box (p. )).

Solution → Run Calculation → Input Summary...

Figure . : The Input Summary Dialog Box

The steps are as follows:

. Select the information you would like to see in the report (Models, Boundary Conditions, Solver Controls,

and/or Material Properties) in the Report Options list.

. To print the information to the ANSYS Fluent console window, click the Print button.To save the inform-

ation to a text file, click the Save... button and specify the filename in the resulting Select File dialog box.

You can print several reports of memory and processor usage from the Parallel ribbon tab.

... Processor Information

... Memory Information

... Process and Model Timers

You can print out a table summarizing the processor usage on each machine that has compute processes

spawned for the current session by clicking CPU Info and selecting CPU Info in the Parallel ribbon

tab (System group box). For example, if processes have been spawned on three machines, a table

similar to the following is displayed:

---------------------------------------------------------------------------------------

| CPU                                  | System Mem (GB)

Hostname            | Sock x Core  Clock (MHz)  Load       | Total        Available

host23              |  x , HT    . . | . .

host24              |  x , HT    . . | . .

host25              |  x , HT    . . | . .

Total               |           -            -          | . .

Under CPU:

Sock x Core

displays the number of processor sockets, number of cores per socket, and whether hyper-threading is

used.

Clock (MHz)

is the processor speed.

Load

is the work load on the machine.

Under System Mem (GB):

Total

is the total system memory on the machine.

Available

is the available system memory on the machine.

You can print out information about the GPUs available on the machine by clicking CPU Info and se-

lecting GPU Info in the Parallel ribbon tab (System group box). If your machine has one or more

suitable GPUs present, you can use these to accelerate parallel processing computations as described

in Using General Purpose Graphics Processing Units (GPGPUs) With the Algebraic Multigrid (AMG)

CUDA visible GPUs on host01

CUDA runtime version

Driver version

Number of GPUs

. Quadro K2100M

SMs

System Resource Usage

. GHz

. GBytes

SMs

. GHz

. GBytes

You can print out tables summarizing memory usage by node and by host by clicking CPU Info and

selecting Memory Usage in the Parallel ribbon tab (System group box).

| Virtual Mem Usage (GB)|

ID     | Current      Peak     | Page Faults

host   | . . | .667e+

n0     | . . | .229e+

n1     | . . | .988e+

n2     | . . | .318e+

n3     | . . | .999e+

Total  | . . | .12e+

| Virtual Mem Usage (GB)    | System Mem (GB)

Hostname            | Current      Peak         |

host01              | . . | .

Total               | . . |

Under Virtual Mem Usage (GB):

Current

is the virtual memory usage at the time the report is generated.

Peak

is the peak virtual memory usage.

(Linux only) Under Resident Mem Usage (GB):

Current

is the resident memory usage at the time the report is generated.

Peak

is the peak resident memory usage.

Page Faults

is the number of page faults that have occurred.

You can use these commands to plan ANSYS Fluent jobs and machines accordingly. They may also be

useful to diagnose performance problems.

You can print out detailed information about the CPU timings for the current session as well as solver

timings by clicking CPU Info and selecting Time Usage in the Parallel ribbon tab (System group box).

The solver timings presented are described in Checking Parallel Performance (p. ).

| CPU Time Usage (Seconds)

ID     | User         Kernel   Elapsed

host   | . . .

n0     | . . .

n1     | . . .

n2     | . . .

n3     | . . .

Total  | . . -

Model Timers (Host)

Other Models Time:                                  . sec

Total Time:                                         . sec

Model Timers

Performance Timer for  iterations on  compute nodes

Average wall-clock time per iteration:              . sec

Global reductions per iteration:                        ops

Global reductions time per iteration:               . sec (.%)

Message count per iteration:                          messages

Data transfer per iteration:                        . MB

LE solves per iteration:                                 solves

LE wall-clock time per iteration:                   . sec (.%)

LE global solves per iteration:                          solves

LE global wall-clock time per iteration:            . sec (.%)

LE global matrix maximum size:

AMG cycles per iteration:                           . cycles

Relaxation sweeps per iteration:                       sweeps

Relaxation exchanges per iteration:                    exchanges

Total wall-clock time:                              . sec

Total CPU time:                                    . sec

Chapter : Field Function Definitions

You must select flow variables for a number of tasks in ANSYS Fluent. The values are computed and

placed in temporary memory that is allocated for storing the results for each cell. For example, the

Compute command associated with a dialog box that contains the field variable drop-down list calculates

the values of the selected function and places them into temporary storage.

Node, Cell, and Facet Values (p. ) and Velocity Reporting Options (p. ) provide some general in-

formation related to the field variables. In Field Variables Listed by Category (p. ), the variables are

listed by category in Table . : Pressure and Density Categories (p. ) – Table . : Acoustics

Category (p. ). These tables will also indicate when each variable will be available. Alphabetical Listing

of Field Variables and Their Definitions (p. ) contains an alphabetical listing of the variables along

with their definitions. All variables appear as they would in the variable selection drop-down lists that

are contained in many of the ANSYS Fluent dialog boxes. Custom Field Functions (p. ) explains how

you can calculate your own field function.

.. Node, Cell, and Facet Values

..Velocity Reporting Options

.. Field Variables Listed by Category

.. Alphabetical Listing of Field Variables and Their Definitions

.. Custom Field Functions

For the following discussion,“surface” refers to a collection of facets, lines or points that are created

and manipulated in the Setting Up Domain ribbon tab. In most cases, these surfaces are created by

computing intersections of constant isovalues with the domain cells or with existing surfaces.

... Cell Values

... Node Values

... Facet Values

ANSYS Fluent stores most variables in cells. For postprocessing, the entire region contained within the

cell has this value. A surface cell value is the value of the cell that has been intersected by a surface

facet or line, or that contains a surface point. Since surface facets and lines are created from the inter-

section of isovalues and the existing mesh cells, this is a unique definition. Typically, the cell value on

a boundary is the value in the cell adjacent to the boundary. For face-only functions like Wall Shear

Stress, the cell value is the area-weighted average from the face values that define that cell as c0.

This value is used for the cell values of postprocessing surfaces. But for boundary faces, the cell value

actually displays/uses the exact face value.

Node values are explicitly defined or obtained by weighted averaging of the cell data. Various

boundary conditions impose values of field variables at the domain boundaries, so mesh node values

on these boundary zones are obtained by simple averaging of the adjacent boundary face data. In

addition, for several variables (for example, node coordinates or node displacements for the structural

model) explicit node values are available at all nodes.

Computation of node values is performed in two steps:

. Values at all nodes are initialized to the weighted average of the surrounding cell values.The weights are

the inverses of the cell volumes that neighbor the nodes.

. At boundaries, these node values are overwritten with the simple average of the boundary face values.

Variables for which explicit node values are available at boundaries are indicated by bnv in Table . :

Pressure and Density Categories (p. ) – Table . : Acoustics Category (p. ).

For example, in Figure . : Computing Node Values (p. ), the value at node

will be computed

from the weighted average of the values in the surrounding cells (

—

). The value at node

will

be computed from the simple average of the boundary faces (

and

) if there are explicit

boundary values available for the variable in question.

Figure . : Computing Node Values

....Vertex Values for Points That Are Not Mesh Nodes

The values of the nodes on surfaces are linearly interpolated from the mesh node data. For zone

surfaces, the nodes on the surface and the zone correspond; therefore, the values are identical. For

surfaces that are not zone surfaces (for example, isosurfaces, plane surfaces, and so on), the node

values are interpolated from mesh nodes on the cell faces intersected by the postprocessing surface.

For point surfaces and structural point surfaces, the value is interpolated from all the mesh nodes of

the cell containing the point.

Facets can be created on preprocessing surfaces and postprocessing surfaces.

Field Function Definitions

.... Facet Values on Zone Surfaces

The interior facets on a zone surface are associated with two cells (c0 and c1). The values of a specified

variable on such facets are computed as the arithmetic average of the two cell values of the selected

variable.

The boundary facet values of a primary field variables on a zone surface are taken from the specified

boundary conditions. The boundary values of dependent variables are computed from the adjacent

cell values (versus using the value of the primary variable specified at the boundary). For exact values

of dependent variables at the boundaries, define a custom field function specifying the boundary

conditions as the primary variables. For more information on custom field functions, see Custom Field

.... Facet Values on Postprocessing Surfaces

Each facet on a postprocessing surface is associated with a cell. The values of a specified variable on

facets are the same as the cell values of the selected variable in the associated cells (this includes iso

surfaces, planes, lines, points, rakes, quadric, and so on).

The following methods are available for reporting velocities:

Cartesian velocities:

These velocities are based on the Cartesian coordinate system used by the geometry. To report

Cartesian velocities, select X Velocity, Y Velocity, or Z Velocity. This is the most common type of

velocity reported.

Cylindrical velocities:

These velocities are the axial, radial, and tangential components based on the following coordinate

systems:

– For axisymmetric problems, in which the rotation axis must be the  axis, the  direction is the axial dir-

ection and the  direction is the radial direction. (If you model axisymmetric swirl, the swirl direction is

the tangential direction.)

– For 2D problems involving a single cell zone, the  direction is the axial direction, and its origin is specified

in the Fluid Dialog Box (p. ).

– For 3D problems involving a single cell zone, the coordinate system is defined by the rotation axis and

– For problems involving multiple zones (for example, multiple reference frames or sliding meshes), the

coordinate system is defined by the rotation axis specified in the Fluid Dialog Box (p. ) (or Solid Dialog

Box (p. )) for the “reference zone”.The reference zone is chosen in the Reference Values Task Page (p. ),

as described in Reference Values (p. ). Recall that for 2D problems, you will specify only the axis origin;

the  direction is always the axial direction.

For all of the above definitions of the cylindrical coordinate system, positive radial velocities point

radially out from the rotation axis, positive axial velocities are in the direction of the rotation axis

Velocity Reporting Options

vector, and positive tangential velocities are based on the right-hand rule using the positive rotation

axis.

To report cylindrical velocities, select Axial Velocity, Radial Velocity, and so on. Figure . : Cylindrical

axis.

Velocity Components in 3D, 2D, and Axisymmetric Domains (p. ) illustrates the cylindrical velocities

available for different types of domains. For 3D problems, you can report axial, radial, and tangential

velocities. For 2D problems, radial and tangential velocities are available. For axisymmetric problems,

you can report axial and radial velocities, and, if you are modeling axisymmetric swirl, you can also

report the swirl velocity (which is equivalent to the tangential velocity).

Relative velocities:These velocities are based on the coordinate system and motion of a moving reference

frame.They are useful when you are modeling your flow using a moving reference frame, a mixing plane,

multiple reference frames, or sliding meshes. (See Modeling Flows with Moving Reference Frames (p. )

for information about modeling flow in moving zones.) To report relative velocities, select Relative X Velocity,

Relative Y Velocity, Relative Radial Velocity, and so on. (Note that you can report relative velocities for

both Cartesian and cylindrical components.)

If you are using a single moving reference frame, the relative velocity values will be reported with

respect to the moving frame. If you are using multiple reference frames, mixing planes, or sliding

meshes, you will need to specify the frame to which you want the velocities to be relative by

choosing the appropriate cell zone as the Reference Zone in the Reference Values Task Page (p. )

(see Reference Values (p. )). The axis of rotation for each cell zone is defined in the associated

Fluid Dialog Box (p. ) or Solid Dialog Box (p. ). (See Specifying the Rotation Axis (p. ) or Spe-

cifying the Rotation Axis (p. ) for details.)

Note that if your problem does not involve any moving zones, relative and absolute velocities will

be equivalent.

Note that relative velocities can also be used to compute stagnation quantities (total pressure and total

temperature), and that the cylindrical coordinate systems described in the second item above are used

for defining the Axial Coordinate and Radial Coordinate as well.

The field variables available in each category are summarized in the following tables:

Table . : Pressure and Density Categories (p. )

Table . : Velocity Category (p. )

Table . : Temperature, Radiation, and Solidification/Melting Categories (p. )

Table . : Turbulence Category (p. )

Table . : Species, Reactions, Pdf, and Premixed Combustion Categories (p. )

Table . : NOx, Soot, and Steady|Unsteady Statistics Categories (p. )

Table . : Phases, Discrete Phase Model, Granular Pressure, Granular Temperature, and Wall Film

Categories (p. )

Table . : Properties Category (p. )

Table . : Eulerian Wall Film Category (p. )

Table . : Sensitivities Category (p. )

Table . : Wall Fluxes, User Defined Scalars, and User Defined Memory Categories (p. )

Table . : Mesh Category (Turbomachinery-Specific Variables) (p. )

Table . : Residuals Category (p. )

Table . : Derivatives Category (p. )

Table . : Potential Category (p. )

Table . : Acoustics Category (p. )

Table . : Structure Category (p. )

In these tables, the following restrictions apply to marked variables:

available only for 2D flows

2d

available only for 2D axisymmetric flows (with

or without swirl)

2da

available only for 2D axisymmetric swirl flows

2dasw

available only for 3D flows

3d

available only with data from the adjoint solver

adj

available only for adjoint calculations that use the

dissipation stabilization scheme

adis

available only when the energy adjoint equation is

solved

aen

available only with the Aungier-Redlich-Kwong

real gas model

ark

available only when created using the Acoustic

Sources FFT Dialog Box (p. ) or related text

commands

asfft

available only with the acoustics wave

equation model

awe

available only for broadband noise source

models

bns

node values available at boundaries

bnv

available only for compressible flow

cmp

available only in the density-based solvers

cpl

Field Variables Listed by Category

available only for cell values (Node Values

option turned off)

cv

available only when the DDPM model is used

ddpm

available when the turbulence model includes

the DES turbulence model

des

not available with full multicomponent

diffusion

dil

available only for dynamic mesh calculations

dm

available only when the discrete ordinates

radiation model is used

do

available only for coupled discrete phase

calculations

dpm

available only when Mean Values are enabled in

the DPM dialog box

dpmean

available only when RMS Values are enabled in the

DPM dialog box

dprms

dpm

dpmean

dprms

available only when the discrete transfer

dtrm

available only with the Ffowcs Williams and

Hawkings acoustics model

fwh

available only for energy calculations

e

available only with the Electrochemical

Reactions model

echem

available only with the EDC model for

turbulence-chemistry interaction

edc

available only when the Eulerian multiphase

model is used

emm

available only with the Eulerian Wall Film

model

ewf

available only with the enhanced wall

treatment

ewt

available for face values

fv

available only if a granular phase is present

gran

available only when the mixture contains water

h2o

available only for hanging node adaption

hn

available only when the ideal gas law is

enabled for density

id

available when one of the -  turbulence

models is used

ke

available when the -

kklo

available when one of the -

turbulence

kw

available when the LES turbulence model is

used

les

available only when the Lagrangian wall film

lwf

available only when the Monte Carlo model is

used

mc

available only when the melting and

solidification model is used

melt

available only when the multiphase mixture

mix

available only for multiphase models

mp

available only for porous cell zones with the

non-equilibrium thermal model enabled

netm

available only for NOx calculations

nox

uses explicit node value function

nv

uses explicit node value solutions

nvs

available only when overset meshing is used

os

available only when the P- radiation model

is used

nox

nv

nvs

os

is used

p1

available only for non-premixed combustion

pdf

available only for premixed combustion

pmx

available only when the potential equation is

solved

pot

available only for partially premixed

combustion calculations

ppmx

available only when the Rosseland radiation

r

available only for radiation heat transfer

rad

available only for finite-rate reactions

rc

available only for the real gas models

rg

available when the Reynolds stress turbulence

rsm

available only when the surface-to-surface

s2s

available when the Spalart-Allmaras turbulence

sa

sas

the Stress-Blended Eddy Simulation (SBES)

turbulence model

sbes

the Shielded Detached Eddy Simulation (SDES)

sdes

available only in the pressure-based solver

seg

available only when the solar model is used

sol

available only for soot calculations

soot

available only for species calculations

sp

available only for surface reactions

sr

available when the Transition SST model is

used

sst

available only with data sampling for transient

statistics

stat

available only for stiff chemistry calculations

stcm

available only when a structural model is

selected

strc

available only for turbulent flows

t

available only when thin walls are present

th

stcm

selected

strc

t

th

available only for transient flow calculations

trn

available only when a turbomachinery

topology has been defined

turbo

available only when a user-defined memory is

used

udm

available only when a user-defined scalar is

used

uds

available only for viscous flows

v

available only for VOF-to-DPM model transition

vof-dpm

Table . : Pressure and Density Categories

Variable

Category

Static Pressure (bnv)

Pressure...

Absolute Pressure (bnv)

Total Pressure (bnv)

Relative Total Pressure

Capillary-Pressure (emm)

Density

Density...

Variable

Category

Table . : Velocity Category

Variable

Category

Velocity Magnitude (bnv)

Velocity...

X Velocity (bnv)

Y Velocity (bnv)

Z Velocity (3d, bnv)

Swirl Velocity (2dasw, bnv)

Axial Velocity (2da or 3d)

Stream Function (2d)

Mach Number (id or rg)

Relative Velocity Magnitude (bnv)

Relative X Velocity (bnv)

Relative Y Velocity (bnv)

Relative Z Velocity (3d, bnv)

Relative Axial Velocity (2da)

Relative Radial Velocity (2da)

Relative Swirl Velocity (2dasw, bnv)

Relative Tangential Velocity

Relative Mach Number (id or rg)

Mesh X-Velocity (nv)

Mesh Y-Velocity (nv)

Mesh Z-Velocity (3d, nv)

Relative Velocity Angle

Vorticity Magnitude (v)

Variable

Category

Helicity (v, 3d)

X-Vorticity (v, 3d)

Y-Vorticity (v, 3d)

Z-Vorticity (v, 3d)

Cell Reynolds Number (v)

Cell Convective Courant Number (seg)

Cell Acoustic Courant Number (cmp, seg)

Category

Preconditioning Reference Velocity (cpl)

Table . : Temperature, Radiation, and Solidification/Melting Categories

Variable

Category

Static Temperature (e, bnv, nv)

Temperature...

Total Temperature (e, nv)

Sensible Enthalpy (e, nv)

Enthalpy (e, nv)

Relative Total Temperature (e)

Rothalpy (e, nv)

Fine Scale Temperature (edc,e)

Wall Temperature (fv, e, v)

Wall Temperature (Thin) (th, fv, e, v)

Wall Adjacent Temperature (fv, e)

Total Enthalpy (e)

Total Enthalpy Deviation (e)

Entropy (e)

Total Energy (e)

Internal Energy (e)

Non-Equilibrium Thermal Model Source (e,

netm)

Absorption Coefficient (r, p1, do, mc, or dtrm)

Radiation...

Scattering Coefficient (r, p1, do, or mc)

Variable

Category

Refractive Index (do or mc)

Radiation Temperature (p1,do, or mc)

Incident Radiation (p1, do, or mc)

Incident Radiation (Band n) (p1 (non-gray),

do (non-gray), or mc (non-gray))

Volumetric Absorbed Radiation (p1, do, or

mc)

Volumetric Emitted Radiation (p1, do, or mc)

Wall Irradiation Flux.Normalized Std Devi-

ation (mc)

Radiation Intensity.Normalized Std Devi-

ation (mc)

Surface Cluster ID (fv, s2s)

Liquid Fraction (melt)

Solidification/ Melting

Contact Resistivity (fv, melt)

X Pull Velocity (melt (if calculated))

Y Pull Velocity (melt (if calculated))

Z Pull Velocity (melt (if calculated), 3d)

Axial Pull Velocity (melt (if calculated), 2da)

Radial Pull Velocity (melt (if calculated), 2da)

Swirl Pull Velocity (melt (if calculated), 2dasw)

Table . : Turbulence Category

Variable

Category

Variable

Category

Turbulent Kinetic Energy (k) (ke, kw, kklo,

sst, rsm, les; sbes, sdes, bnv, nv, or emm)

Turbulence...

Laminar Kinetic Energy (kklo)

Total Fluctuation Energy (kklo)

Turbulent Intensity (ke, kw, kklo, sst, rsm, les,

sbes, sdes)

Intermittency (sst, kw, sas, des, sbes, sdes)

Variable

Category

Intermittency Effective (sst, sbes (with

Transition SST only), sdes (with Transition SST

only))

Momentum Thickness Re (sst, sbes (with

only))

Geometric Roughness Height (sst, sbes (with

only))

UU Reynolds Stress (rsm; emm)

VV Reynolds Stress (rsm; emm)

WW Reynolds Stress (rsm; emm)

UV Reynolds Stress (rsm; emm)

UW Reynolds Stress (rsm, 3d; emm)

VW Reynolds Stress (rsm, 3d; emm)

Resolved UV Reynolds Stress (sas, des, sbes,

sdes, les)

Resolved UW Reynolds Stress (sas, des, sbes,

sdes, les)

Resolved VW Reynolds Stress (sas, des, sbes,

sdes, les)

Turbulent Dissipation Rate (Epsilon) (ke, kw,

kklo, sst, sbes, sdes, or rsm; bnv (k-epsilon

model only), nv (k-epsilon model only), or

emm)

Specific Dissipation Rate (Omega) (kw, kklo,

sst, sbes, sdes, rsm)

Production of k (ke, kw, kklo, sst, rsm, les;

emm)

Production of laminar k (kklo)

Modified Turbulent Viscosity (sa, des)

Turbulent Viscosity (sa, ke, kw, kklo, sst, sbes,

sdes, rsm, sas, des, les)

Turbulent Viscosity (large-scale) (kklo)

Turbulent Viscosity (small-scale) (kklo)

Variable

Category

Effective Viscosity (sa, ke, kw, kklo, sst, sbes,

sdes, rsm, des; emm)

Variable

Category

Turbulent Viscosity Ratio (ke, kw, kklo, sst,

sbes, sdes, rsm, sa, des, les; emm)

LES Subgrid Turbulent Viscosity (les)

Subgrid Kinetic Energy (les)

Subgrid Turbulent Viscosity (les)

Subgrid Turbulent Viscosity Ratio (les)

Subgrid Effective Viscosity (les)

Subgrid Filter Length (les)

Subgrid Test-Filter Length (les)

Subgrid Dissipation Rate (les)

Subgrid Dynamic Viscosity Const (les)

Subgrid Dynamic Prandtl Number (les)

Subgrid Dynamic Sc of Species (les)

Subtest Kinetic Energy (les)

Effective Thermal Conductivity (t, e)

Effective Prandtl Number (t, e)

Wall Ystar (fv, ke, kw, kklo, sst, sbes, sdes, rsm,

les)

Wall Yplus (fv, t)

Turbulent Reynolds Number (Re_y) (ke, kw,

kklo, sst, sbes, sdes, rsm; ewt)

Relative Length Scale (DES) (des)

DES TKE Dissipation Multiplier (des)

Curvature Correction Function fr (sa, ke, kw,

sst, sbes, sdes, sas, des)

Shielding Function for SBES or SDES (sbes,

sdes)

Normalized Q Criterion (des, sas, les, sbes,

sdes)

Variable

Category

Q Criterion (des, sas, les, sbes, sdes)

Lambda  Criterion (des, sas, les, sbes, sdes)

Table . : Species, Reactions, Pdf, and Premixed Combustion Categories

Variable

Category

Mass fraction of species-n  (sp, pdf, or

ppmx; nv)

Species...

Mole fraction of species-n  (sp, pdf, or

ppmx)

Molar Concentration of species-n  (sp, pdf,

or ppmx)

Lam Diff Coef of species-n  (sp, dil)

Eff Diff Coef of species-n  (t, sp, dil)

Thermal Diff Coef of species-n  (sp)

Enthalpy of species-n  (sp)

species-n Source Term (rc, cpl)

Surface Deposition Rate of species-n  (sr)

Surface Coverage of species-n  (sr)

Porous Deposition Rate of species-n  (sr)

Relative Humidity (sp, pdf, or ppmx; h2o)

Time Step Scale (sp, stcm)

Fine Scale Mass fraction of species-n

(edc)

Cell Time Scale (edc)

EDC Cell Volume Fraction (edc)

DRG Reduced Number of Species (sp)

Reactor Net Zone ID (sp)

Reactor Net Temperature (sp)

(sp)

Surface Corrosion Rate of species-n

(echem)

Variable

Category

Rate of Reaction-n (rc)

Reactions...

Kinetic Rate of Reaction-n (rc)

Turbulent Rate of Reaction-n (rc, t)

Heat of Reaction (e, rc)

Net Reaction Rate of Species-n  (edc, stcm)

DRG Reduced Number of Reactions (sp)

Echem Reaction Rate of Reaction-n (echem)

Mean Mixture Fraction (pdf or ppmx; nv)

Pdf...

Secondary Mean Mixture Fraction (pdf or

ppmx; nv)

Mixture Fraction Variance (pdf or ppmx; nv)

Secondary Mixture Fraction Variance (pdf or

ppmx; nv)

Fvar Prod (pdf or ppmx)

Fvar2 Prod (pdf or ppmx)

Scalar Dissipation (pdf or ppmx)

Heat Release Rate (pdf or ppmx)

PDF Table Adiabatic Enthalpy (pdf or ppmx)

PDF Table Heat Loss/Gain (e, pdf or ppmx)

Progress Variable (pmx or ppmx; nv)

Premixed Combustion...

Progress Variable Variance (ppmx; nv)

Scalar Mass Fraction of species-n  (ppmx)

Forward Reaction Rate of PDF scalar-n

(ppmx)

Reverse Reaction Rate of PDF scalar-n

(ppmx)

Damkohler Number (pmx or ppmx)

Stretch Factor (pmx or ppmx)

Turbulent Flame Speed (pmx or ppmx)

Static Temperature (pmx or ppmx)

Variable

Category

(ppmx)

Variable

Category

Product Formation Rate (pmx or ppmx)

Laminar Flame Speed (pmx or ppmx)

Critical Strain Rate (pmx or ppmx)

Adiabatic Flame Temperature (pmx or ppmx)

Unburnt Fuel Mass Fraction (pmx or ppmx)

Table . : NOx, Soot, and Steady|Unsteady Statistics Categories

Variable

Category

Mass fraction of NO (nox)

NOx...

Mass fraction of HCN (nox)

Mass fraction of NH3 (nox)

Mass fraction of N2O (nox)

Mole fraction of NO (nox)

Mole fraction of HCN (nox)

Mole fraction of NH3 (nox)

Mole fraction of N2O (nox)

NO Density (nox)

HCN Density (nox)

NH3 Density (nox)

N2O Density (nox)

Variance of Temperature (nox)

Variance of Species (nox)

Variance of Species  (nox)

Rate of NO (nox)

Rate of Thermal NO (nox)

Rate of Prompt NO (nox)

Rate of Fuel NO (nox)

Rate of N2OPath NO (nox)

Variable

Category

Rate of Reburn NO (nox)

Rate of SNCR NO (nox)

Rate of USER NO (nox)

Average Number of Particles in Soot Aggreg-

ate (soot)

Soot...

Concentration of soot species-n (soot)

Mass fraction of soot (soot)

Mass fraction of Nuclei (soot)

Mole fraction of soot (soot)

Normalized Concentration of Nuclei (soot)

Normalized Soot Aggregation Moments

(soot)

Normalized soot moments (soot)

Primary Particle Diameter (soot)

Rate of Coagulation (soot)

Rate of Nuclei (soot)

Rate of Nucleation (soot)

Rate of Oxidation (soot)

Rate of Soot (soot)

Rate of Soot Mass Nucleation (soot)

Rate of Surface Growth (soot)

Site fraction of soot species-n (soot)

Soot Density (soot)

Soot Mean Diameter (soot)

Soot Surface Area (soot)

Soot Volume fraction (soot)

Accum DPM Parcels in Cell (dpm, stat)

Steady|Unsteady DPM

Statistics...

Accum DPM Particles in Cell (dpm, stat)

Mean DPM n (dpm, stat)

Variable

Category

RMS DPM n (dpm, stat)

Mean n (stat)

Steady|Unsteady Statist-

ics...

Mean- cff_n (stat)

RMSE n (stat)

RMSE- cff_n (stat)

Table . : Phases, Discrete Phase Model, Granular Pressure, Granular Temperature, and Wall

Film Categories

Variable

Category

Phase Interaction...

Mass Transfer Rate n

Saturation Temperature n

Latent Heat n

Volume fraction (mp)

Phases...

Lump ID (vof-dpm)

Lump Detection...

Lump Diameter (vof-dpm)

Lump Density (vof-dpm)

Lump Asph. by Rad. Std. Dev. (vof-dpm)

Lump Asph. by Orthogonality (vof-dpm)

Lump X, Y, Z Coordinate (vof-dpm)

Lump Temperature (vof-dpm, e)

Lump Enthalpy (vof-dpm, e)

Lump Pressure (vof-dpm, e)

DPM Erosion Rate (Generic) (dpm, cv, fv)

Discrete Phase Variables...

DPM Erosion Rate (Finnie) (dpm, cv, fv)

DPM Erosion Rate (McLaury) (dpm, cv, fv)

DPM Erosion Rate (Oka) (dpm, cv, fv)

DPM Erosion Rate (Wall Shear)  (dpm, cv, fv,

gran)

DPM Accretion (dpm, cv, fv)

DPM Volume Fraction (dpm, dpmean)

Variable

Category

DPM Parcels in Cell (dpm, dpmean)

DPM Particles in Cell (dpm, dpmean)

DPM Number Density (dpm, dpmean)

DPM Collision Rate (dpm)

DPM X Velocity (dpm, dpmean)

DPM Y Velocity (dpm, dpmean)

DPM Z Velocity (dpm, dpmean)

DPM Diameter (dpm, dpmean)

DPM Density (dpm, dpmean)

DPM Temperature (dpm, dpmean)

DPM Specific Heat (dpm, dpmean)

DPM D20 (dpm, dpmean)

DPM D30 (dpm, dpmean)

DPM D32 (dpm, dpmean)

DPM D43 (dpm, dpmean)

DPM Granular Temperature (ddpm, gran)

DPM Conc of <component>  (dpm, dpmean,

sp)

DPM RMS X Velocity (dpm, dprms)

DPM RMS Y Velocity (dpm, dprms)

DPM RMS Z Velocity (dpm, dprms)

DPM RMS Diameter (dpm, dprms)

DPM RMS Temperature (dpm, dprms)

DPM Absorption Coefficient (dpm, rad)

DPM Emission (dpm, rad)

DPM Scattering (dpm, rad)

DPM Concentration (dpm)

DPM Wall X Force (dpm)

Variable

Category

DPM Wall Y Force (dpm)

DPM Wall Z Force (dpm)

DPM Wall Normal Pressure (dpm)

DPM Mass Source (dpm)

Discrete Phase Sources...

DPM X Momentum Source (dpm)

DPM Y Momentum Source (dpm)

DPM Z Momentum Source (dpm, 3d)

DPM Swirl Momentum Source (dpm, 2dasw)

DPM Sensible Enthalpy Source (dpm, e, rc)

DPM Enthalpy Source (dpm, e)

DPM Burnout (dpm, sp, e)

DPM Evaporation/Devolatilization (dpm, sp,

e)

DPM species-n Source (dpm, sp, e)

Granular Pressure (emm, gran)

Granular Pressure...

Granular Temperature (emm, gran)

Granular Temperature...

Wall Film Height (dpm, lwf)

Wall Film...

Wall Film Impingement Mass Flux (dpm, lwf)

Wall Film Face Pressure (dpm, lwf)

Wall Film Mass (dpm, lwf)

Wall Film Temperature (dpm, lwf)

Wall Film Heat Flux (dpm, lwf)

Wall Film X-Velocity (dpm, lwf)

Wall Film Y-Velocity (dpm, lwf)

Wall Film Z-Velocity (dpm, lwf, 3d)

Wall Film Velocity Magnitude (dpm, lwf)

Wall Leidenfrost Temperature (dpm, lwf)

Wall Coverage (dpm, lwf)

Variable

Category

Film Mass Fraction of material-i  (dpm,

lwf)

Variable

Category

lwf)

Table . : Properties Category

Variable

Category

Molecular Viscosity (v)

Properties...

Diameter (mix, emm)

Granular Conductivity (mix, emm, gran)

Thermal Conductivity (e, v)

Specific Heat (Cp) (e)

Specific Heat Ratio (gamma) (id)

Gas Constant (R) (id or rg)

Molecular Prandtl Number (e, v)

Mean Molecular Weight (seg, pdf)

Sound Speed (id or rg)

Compressibility Factor (rg)

Reduced Temperature (ark)

Reduced Pressure (ark)

Critical Temperature (ark, spe)

Critical Pressure (ark, spe)

Acentric Factor (ark,spe)

Critical Specific Volume (ark,spe)

Spinodal Temperature (ark)

Electric Conductivity (pot)

Table . : Eulerian Wall Film Category

Variable

Category

Film Thickness (3d, ewf)

Eulerian Wall Film...

Film Mass (3d, ewf)

Film Temperature (3d, ewf)

Film X-Velocity (3d, ewf)

Variable

Category

Film Y-Velocity (3d, ewf)

Film Z-Velocity (3d, ewf)

Film Velocity Magnitude (3d, ewf)

Film Coverage (3d, ewf)

Film Effective Pressure (3d, ewf)

Film Surface X-Velocity (3d, ewf)

Film Surface Y-Velocity (3d, ewf)

Film Surface Z-Velocity (3d, ewf)

Film Surface Velocity Magnitude (3d, ewf)

Film Surface Temperature (3d, ewf)

Film Passive Scalar (3d, ewf)

Film Courant Number (3d, ewf)

Film Weber Number (3d, ewf)

Film Stripped Mass (3d, ewf)

Film Stripped Diam (3d, ewf)

Film DPM Mass Source (3d, ewf, dpm)

Film DPM Energy Source (3d, ewf, dpm)

Film DPM X-Momentum Source (3d, ewf,

dpm)

Film DPM Y-Momentum Source (3d, ewf,

dpm)

Film DPM Z-Momentum Source (3d, ewf,

dpm)

Film X-Momentum Source (3d, ewf)

Film Y-Momentum Source (3d, ewf)

dpm)

dpm)

dpm)

Film Separated Mass (3d, ewf)

Film Separated Diam (3d, ewf)

Film Separation Rate (3d, ewf)

Film Phase Change Rate  (3d, ewf)

Variable

Category

Film Outflow Mass (3d, ewf)

Film Secondary Phase Mass (3d, ewf)

Film Secondary Phase Collection Coef (3d,

ewf)

Table . : Sensitivities Category

Variable

Category

Magnitude of Sensitivity to Body Forces

(Cell Values) (adj)

Sensitivities...

Sensitivity to Body Force X-Component (Cell

Values) (adj)

Sensitivity to Body Force Y-Component (Cell

Sensitivity to Body Force Z-Component (Cell

Values) (adj, 3d)

Sensitivity to Mass Sources (Cell Values) (adj)

Sensitivity to Energy Sources (Cell Values)

(adj, aen)

Artificial Dissipation (adj, adis)

Sensitivity to Viscosity (adj)

Shape Sensitivity Magnitude (adj)

Normal Shape Sensitivity (adj)

Normal Optimal Displacement (adj)

log10(Shape Sensitivity Magnitude) (adj)

Shape Sensitivity X-Component (adj)

Shape Sensitivity Y-Component (adj)

Shape Sensitivity Z-Component (adj, 3d)

Sensitivity to Boundary X-Velocity (adj)

Sensitivity to Boundary Y-Velocity (adj)

Sensitivity to Boundary Z-Velocity (adj, 3d)

Sensitivity to Boundary Pressure (adj)

Variable

Category

Sensitivity to Boundary Temperature (adj,

aen)

Sensitivity to Boundary Heat Flux (adj, aen)

Sensitivity to Flow Blockage (adj)

Adjoint Local Solution Marker (adj)

Table . : Wall Fluxes, User Defined Scalars, and User Defined Memory Categories

Variable

Category

Wall Shear Stress (v, emm, fv)

Wall Fluxes...

Variable

Category

X-Wall Shear Stress (v, emm, fv)

Y-Wall Shear Stress (v, emm, fv)

Z-Wall Shear Stress (v, 3d, emm, fv)

Axial-Wall Shear Stress (2da, fv)

Radial-Wall Shear Stress (2da, fv)

Swirl-Wall Shear Stress (2dasw, fv)

Skin Friction Coefficient (v, emm, fv)

Total Surface Heat Flux (e, v, fv)

Radiation Heat Flux (fv, rad)

Solar Heat Flux (sol, fv)

Absorbed Radiation Flux (Band-n) (do, fv)

Absorbed Visible Solar Flux (sol, fv)

Absorbed IR Solar Flux (sol, fv)

Reflected Radiation Flux (Band-n) (do, fv)

Reflected Visible Solar Flux (sol, fv)

Reflected IR Solar Flux (sol, fv)

Transmitted Radiation Flux (Band-n) (do, fv)

Transmitted Visible Solar Flux (sol, fv)

Transmitted IR Solar Flux (sol, fv)

Beam Irradiation Flux (Band-n) (do, fv)

Variable

Category

Surface Incident Radiation (do, dtrm, or s2s;

fv)

Surface Heat Transfer Coef. (e, v, fv)

Wall Func. Heat Tran. Coef. (e, v, fv)

Wall Adjacent Heat Transfer Coef. (e, fv)

Surface Nusselt Number (e, v, fv)

Surface Stanton Number (e, v, fv)

Scalar-n (bnv, uds)

User Defined Scalars...

Diffusion Coef. of Scalar-n (bnv, uds)

User Memory <n> (bnv, udm)

User Defined Memory...

User Node Memory <n> (bnv, udm)

Table . : Cell Info and Mesh Categories

Variable

Category

Cell Info...

Cell Id

Overset Cell Type (os)

Overset Donor Count (os)

Overset Receptor Count (os)

X-Coordinate (nv)

Mesh...

Y-Coordinate (nv)

Z-Coordinate (3d, nv)

Axial Coordinate (nv)

Mesh...

Angular Coordinate (3d, nv)

Abs. Angular Coordinate (3d, nv)

Variable

Category

Radial Coordinate

X Face Area

Y Face Area

Z Face Area (3d)

2D Cell Volume (2da)

Accumulated Deformation (dpm, dm, fv)

Dynamic Cell Volume

Table . : Mesh Category (Turbomachinery-Specific Variables)

Variable

Category

Meridional Coordinate (nv, turbo)

Mesh...

Abs Meridional Coordinate (nv, turbo)

Spanwise Coordinate (nv, turbo)

Abs (H-C) Spanwise Coordinate (nv, turbo)

Abs (C-H) Spanwise Coordinate (nv, turbo)

Pitchwise Coordinate (nv, turbo)

Abs Pitchwise Coordinate (nv, turbo)

Variable

Category

Boundary Normal Distance

Cell Refine

Table . : Residuals Category

Variable

Category

Mass Imbalance (seg)

Residuals...

Pressure Residual (cpl)

X-Velocity Residual (cpl)

Y-Velocity Residual (cpl)

Z-Velocity Residual (cpl, 3d)

Axial-Velocity Residual (cpl, 2da)

Radial-Velocity Residual (cpl, 2da)

Swirl-Velocity Residual (cpl, 2dasw)

Temperature Residual (cpl, e)

Species-n Residual (cpl, sp)

Time Step (cpl)

Pressure Correction (cpl)

X-Velocity Correction (cpl)

Y-Velocity Correction (cpl)

Z-Velocity Correction (cpl, 3d)

Axial-Velocity Correction (cpl, 2da)

Radial-Velocity Correction (cpl, 2da)

Swirl-Velocity Correction (cpl, 2dasw)

Temperature Correction (cpl, e)

Species-n Correction (cpl, sp)

Table . : Derivatives Category

Variable

Category

Strain Rate (v)

Derivatives...

Variable

Category

dX-Velocity/dx

dY-Velocity/dx

dZ-Velocity/dx (3d)

dAxial-Velocity/dx (2da)

dRadial-Velocity/dx (2da)

dSwirl-Velocity/dx (2dasw)

d species-n/dx (cpl, sp)

dX-Velocity/dy

dY-Velocity/dy

dZ-Velocity/dy (3d)

dAxial-Velocity/dy (2da)

dRadial-Velocity/dy (2da)

dSwirl-Velocity/dy (2dasw)

d species-n/dy (cpl, sp)

dX-Velocity/dz (3d)

dY-Velocity/dz (3d)

dZ-Velocity/dz (3d)

d species-n/dz (cpl, sp, 3d)

dOmega/dx (2dasw)

dOmega/dy (2dasw)

dp-dX (seg)

dp-dY (seg)

dp-dZ (seg, 3d)

dp-dt (trn)

Table . : Potential Category

Variable

Category

Potential...

Current Magnitude

Variable

Category

Faradaic Current Density (echem)

Total Surface Corrosion Rate (echem)

Faradaic Heat Source (echem)

Total Echem Heat Source (echem)

Table . : Acoustics Category

Variable

Category

Surface dpdt RMS (fv, fwh)

Acoustics...

Acoustic Power Level (dB) (bns)

Acoustic Power (bns)

Jet Acoustic Power Level (dB) (bns, 2da)

Jet Acoustic Power (bns, 2da)

Surface Acoustic Power Level (dB) (bns, fv)

Surface Acoustic Power (bns, fv)

Lilley’s Self-Noise Source (bns)

Lilley’s Shear-Noise Source (bns)

Lilley’s Total Noise Source (bns)

LEE Self-Noise X-Source (bns)

LEE Shear-Noise X-Source (bns)

LEE Total Noise X-Source (bns)

LEE Self-Noise Y-Source (bns)

LEE Shear-Noise Y-Source (bns)

LEE Total Noise Y-Source (bns)

LEE Self-Noise Z-Source (bns, 3d)

LEE Shear-Noise Z-Source (bns, 3d)

LEE Total Noise Z-Source (bns, 3d)

Pressure Spectrum Im n (asfft, 3d)

Variable

Category

Pressure Spectrum Re n (asfft, 3d)

Sound Pressure (awe)

Sound Potential (awe)

Sound dP/dt (awe)

Sound WaveEq Model Source (awe)

(awe)

Sound WaveEq Model Source Mask (awe)

Sound Sponge Layer Marker  (awe)

SPL for Octave Band at x Hz (dB) (asfft, 3d)

SPL for /-Octave Band at x Hz (dB) (asfft,

3d)

SPL for Const Width Band n (dB) (asfft, 3d)

Table . : Structure Category

Variable

Category

X Displacement (nvs, strc)

Structure...

Y Displacement (nvs, strc)

Z Displacement (nvs, strc, 3d)

Sigma XX (strc)

Sigma YY (strc)

Sigma XY (strc)

Sigma ZZ (strc, 3d)

Sigma YZ (strc, 3d)

Sigma XZ (strc, 3d)

Below, the variables listed in Table . : Pressure and Density Categories (p. ) – Table . :

Acoustics Category (p. ) are defined. For some variables (such as residuals) a general definition is

given under the category name, and variables in the category are not listed individually. When appro-

priate, the unit quantity is included, as it appears in the Quantities list in the Set Units Dialog Box (p. ).

Abs. Angular Coordinate

(in the Mesh... category) is the absolute value of the Angular Coordinate defined above.

(in the Mesh... category) is the dimensional coordinate in the spanwise direction, from casing to hub. Its

unit quantity is length.

(in the Mesh... category) is the dimensional coordinate in the spanwise direction, from hub to casing. Its

(in the Mesh... category) is the dimensional coordinate that follows the flow path from inlet to outlet. Its

(in the Mesh... category) is the dimensional coordinate in the circumferential (pitchwise) direction. Its unit

quantity is angle.

(in the Pressure... category) is equal to the operating pressure plus the gauge pressure. See Operating

Pressure (p. ) for details. Its unit quantity is pressure.

Absorbed Radiation Flux (Band-n)

(in the Wall Fluxes... category) is the amount of radiative heat flux absorbed by a semi-transparent wall

for a particular band of radiation. Its unit quantity is heat-flux.

Absorbed Visible Solar Flux, Absorbed IR Solar Flux

(in the Wall Fluxes... category) is the amount of solar heat flux absorbed by a semi-transparent wall or

porous jump boundary for a visible or infrared (IR) radiation.

(in the Radiation... category) is the property of a medium that describes the amount of absorption of

thermal radiation per unit path length within the medium. It can be interpreted as the inverse of the mean

free path that a photon will travel before being absorbed (if the absorption coefficient does not vary along

the path).The unit quantity for Absorption Coefficient is length-inverse.

(in the Mesh... category) is the accumulated displacement of the wall surface due to erosion over

time. This variable will appear in the Mesh... category only for erosion dynamic mesh simulations.

See Procedure for the Erosion Coupled with Dynamic Mesh Setup and Solution (p. ) for more in-

Accum Parcels in Cell

(in the Steady | Unsteady DPM Statistics... category)

For steady particle tracking, this is the cumulative count of trajectories that has entered the cell since

the last reset of the unsteady statistics.

For unsteady particle tracking, this is the count of particle parcels that has entered the cell since the last

reset of the unsteady statistics, where each parcel is weighted by the fraction of the respective fluid flow

time step that it actually resides in the cell.

Alphabetical Listing of Field Variables and Their Definitions

Accum Particles in Cell

For steady particle tracking, this is the cumulative sum of trajectories that has entered the cell since the

last reset of the unsteady statistics. Each time a trajectory is counted, the time-constant number of

particles represented by the trajectory in the cell is added to the sum.

For unsteady particle tracking, this is the number of particles in all parcels that have entered the cell

since the last reset of the unsteady statistics. Each parcel is weighted by the fraction of the respective

fluid flow time step that it actually resides in the cell.

(in the Properties... category) is the mixture acentric factor.This property is available when a composition

dependent option is selected for acentric factor in the cases with Aungier-Redlich-Kwong real gas model

and species transport.

(in the Acoustics... category) is the acoustic power per unit volume generated by isotropic turbulence

(see Equation . in the Theory Guide ). It is available only when the Broadband Noise Sources

acoustics model is being used. Its unit quantity is power per volume.

and reported in dB (see Equation . in the Theory Guide ). It is available only when the Broadband

Noise Sources acoustics model is being used.

(in the Cell Info... category) is an integer identifier designating the partition to which a particular cell be-

longs. In problems in which the mesh is divided into multiple partitions to be solved on multiple processors

using the parallel version of ANSYS Fluent, the partition ID can be used to determine the extent of the

various groups of cells.The active cell partition is used for the current calculation, while the stored cell

partition (the last partition performed) is used when you save a case file. See Partitioning the Mesh

Manually and Balancing the Load (p. ) for more information.

(in the Premixed Combustion... category) is the adiabatic temperature of burnt products in a laminar

premixed flame (

in Equation . in the Theory Guide ). Its unit quantity is temperature.

Adjoint Local Solution Marker

(in the Sensitivities... category), intended for expert users who are using the Spatial Stabilization

Scheme (p. ), can be plotted to identify those portions of the flow domain where the stabilized adjoint

solution advancement scheme is applied. It is preferable to plot this with the Node Values disabled in the

Contours dialog box. In this case, the Adjoint Local Solution Marker will take a value between  and .

The Mode Amplitude Cutoff defined in the Stabilized Scheme Settings dialog box defines the lower

bound for cells where the stabilized scheme is applied.

Angular Coordinate

(in the Mesh... category) is the angle between the radial vector and the position vector.The radial vector

is obtained by transforming the default radial vector (y-axis) by the same rotation that was applied to the

default axial vector (z-axis).This assumes that, after the transformation, the default axial vector (z-axis)

becomes the reference axis.The angle is positive in the direction of cross-product between reference axis

and radial vector.

(in the Sensitivities... category) is available when the adjoint dissipation stabilization scheme is enabled

and shows the location and amount of the nonlinear damping that has been introduced to damp the

growth of instabilities that lead to adjoint solution divergence.

Average Number of Particles in Soot Aggregate

(In the Soot… category) is an average number of primary particles in a soot aggregate (

in equation

Equation . in the Fluent Theory Guide).This quantity is available only with the Method of Moments

model.

Axial Coordinate

(in the Mesh... category) is the distance from the origin in the axial direction.The axis origin and (in 3D)

direction is defined for each cell zone in the Fluid Dialog Box (p. ) or Solid Dialog Box (p. ).The axial

direction for a 2D model is always the  direction, and the axial direction for a 2D axisymmetric model is

always the  direction.The unit quantity for Axial Coordinate is length.

Axial Pull Velocity

(in the Solidification/Melting... category) is the axial-direction component of the pull velocity for the

solid material in a continuous casting process. Its unit quantity is velocity.

(in the Velocity... category) is the component of velocity in the axial direction. (See Velocity Reporting

Options (p. ) for details.) For multiphase models, this value corresponds to the selected phase in the

Phase drop-down list. Its unit quantity is velocity.

Axial-Wall Shear Stress

(in the Wall Fluxes... category) is the axial component of the force acting tangential to the surface due to

friction. Its unit quantity is pressure.

Beam Irradiation Flux (Band-b)

(in the Wall Fluxes... category) is specified as an incident heat flux (

) for each wavelength band.

(in the Mesh... category) is an integer that indicates the approximate number of cells from a boundary

zone.

(in the Mesh... category) is the distance of the cell centroid from the closest boundary zone.

zone.

(in the Mesh... category) is the cell volume distribution based on the Boundary Volume, Growth Factor,

and normal distance from the selected Boundary Zones defined in the Boundary (p. ) cell register.

(in the Pressure... category) is the capillary pressure acting on a wetting (secondary) phase in a multiphase

flow through a porous zone. Note that, although this item is available for both non-wetting and wetting

phases, meaningful values are reported only for the wetting phase. See Specifying the Capillary Pres-

sure (p. ) for details.

(in the Adaption... category) is a binary identifier based on whether a cell is the product of cell subdivision

from the hanging node adaption process (value = ) or not (value = ).

(in the Velocity... category) is a ratio of the time step size to the acoustic wave propagation time based

on the cell size.

(in the Velocity... category) is a ratio of the time step size to the convective wave propagation time based

(in the Cell Info... category) is the integer cell element type identification number. Each cell can have one

of the following element types:

triangle

tetrahedron

hexahedron

pyramid

wedge

polyhedra

(in the Mesh... category) is a nondimensional parameter calculated using the normalized angle deviation

method, and is defined as

(.)

where

(.)

where

= angle for an equiangular face or cell (for example,  for a triangle

and  for a square)

A value of  indicates a best case equiangular cell, and a value of  indicates a completely degenerate

cell. Degenerate cells (slivers) are characterized by nodes that are nearly coplanar (collinear in 2D).

Cell Equiangle Skew applies to all elements.

(in the Mesh... category) is a nondimensional parameter calculated using the volume deviation method,

(.)

where optimal-cell-size is the size of an equilateral cell with the same circumradius. A value of

indicates a best case equilateral cell and a value of  indicates a completely degenerate cell. Degen-

erate cells (slivers) are characterized by nodes that are nearly coplanar (collinear in 2D). Cell Equi-

volume Skew applies only to triangular and tetrahedral elements.

Cell Id

(in the Cell Info... category) is a unique integer identifier associated with each cell.

includes quantities that identify the cell and its relationship to other cells.

(in the Adaption... category) is an integer that indicates the number of times a cell has been subdivided

by the adaption process, compared with the original mesh. For example, if one quad cell is split into four

quads, the Cell Refine Level for each of the four new quads will be . If the resulting four quads are split

again, the Cell Refine Level for each of the resulting  quads will be .

(in the Velocity... category) is the value of the Reynolds number in a cell. (Reynolds number is a dimen-

sionless parameter that is the ratio of inertia forces to viscous forces.) Cell Reynolds Number is defined

as

(.)

where  is density,

is velocity magnitude,

is the effective viscosity (laminar plus turbulent), and

is Cell Volume

for 2D cases and Cell Volume

in 3D or axisymmetric cases.

(in the Adaption... category) is the total surface area of the cell, and is computed by summing the area of

the faces that compose the cell.

(in the Mesh... category) is the volume of a cell. In 2D the volume is the area of the cell multiplied by the

unit depth. For axisymmetric cases, the cell volume is calculated using a reference depth of  radian.The

unit quantity of Cell Volume is volume.

(in the Mesh... category) is the change of a cell volume over time.

(in the Mesh... category) is the cell volume over the unsteady cell volume.

2D Cell Volume

(in the Mesh... category) is the two-dimensional volume of a cell in an axisymmetric computation. For an

axisymmetric computation, the 2D cell volume is scaled by the radius. Its unit quantity is area.

(in the Adaption... category) is the maximum volume ratio of the current cell and its neighbors.

(in the Mesh... category) is the distribution of the normal distance of each cell centroid from the wall

boundaries. Its unit quantity is length.

(in the Adaption... category) is the square root of the ratio of the distance between the cell centroid and

cell circumcenter and the circumcenter radius:

(.)

(.)

(in the Cell Info... category) is the integer cell zone identification number. In problems that have more

than one cell zone, the cell zone ID can be used to identify the various groups of cells.

(in the Cell Info... category) is the integer cell zone type ID. A fluid cell has a type ID of , a solid cell has

a type ID of , and an exterior cell (parallel solver) has a type ID of .

(in the Properties... category) is the ratio of the ideal gas density of the fluid divided by the real gas fluid

density in the same flow conditions. Compressibility Factor is defined as

(.)

where  is the compressibility factor,

is the absolute pressure,

is the temperature, and

(the universal gas constant

divided by the molecular weight

). The compress-

ibility factor is available only with the real gas models.

Concentration of soot species-n

(in the Soot... category) is the moles per unit volume of a soot species. Its unit quantity is concentration.

(The name of the soot species will replace soot species-n in Concentration of soot species-n.)

This quantity is available only with the Method of Moments model that uses the Detailed CHEMKIN

Format soot mechanism.

(in the Solidification/Melting... category) is the additional resistance at the wall due to contact resistance.

It is equal to

, where

is the contact resistance,

is the liquid fraction, and  is the cell height

of the wall-adjacent cell.The unit quantity for Contact Resistivity is thermal-resistivity.

, where

(in the Properties... category) is the mixture critical pressure.This property is available when a composition

dependent option is selected for critical pressure in the cases with Aungier-Redlich-Kwong real gas model

(in the Properties... category) is the mixture critical specific volume.This property is available when a

composition dependent option is selected for critical specific volume in the cases with Aungier-Redlich-

Kwong real gas model and species transport.

(in the Premixed Combustion... category) is a parameter that takes into account the stretching and ex-

tinction of premixed flames (

in Equation . in the Theory Guide ). Its unit quantity is time-inverse.

(in the Properties... category) is the mixture critical temperature.This property is available when a com-

position dependent option is selected for critical temperature in the cases with Aungier-Redlich-Kwong

real gas model and species transport

(in the Potential... category) is the magnitude of the electric current vector in the field,

.

(in the Turbulence... category) is the multiplier of the production term when curvature correction is selected

for Spalart-Allmaras or two equation models. See Curvature Correction for the Spalart-Allmaras and Two-

Equation Models in the Fluent Theory Guide for details.

Custom Field Functions...

are scalar field functions defined by you.You can create a custom function using the Custom Field Function

Calculator Dialog Box (p. ). All defined custom field functions will be listed in the lower drop-down list.

See Custom Field Functions (p. ) for details.

(in the Premixed Combustion... category) is a nondimensional parameter that is defined as the ratio of

turbulent to chemical time scales.

includes variables related to density.

Density

(in the Density... category) is the mass per unit volume of the fluid. Plots or reports of Density include

only fluid cell zones. For multiphase models, this value corresponds to the selected phase in the Phase

drop-down list.The unit quantity for Density is density.

(in the Density... category) is the mass per unit volume of the fluid or solid material. Plots or reports of

Density All include both fluid and solid cell zones.The unit quantity for Density All is density.

are the viscous derivatives. For example, dX-Velocity/dx is the first derivative of the  component of ve-

locity with respect to the -coordinate direction.You can compute first derivatives of velocity, angular

velocity, and pressure in the pressure-based solver, and first derivatives of velocity, angular velocity, tem-

perature, and species in the density-based solvers.

(in the Turbulence... category) is available when you keep the temporary solver memory from being freed

using the solve/set/expert text command. It is defined by Equation . in the Theory Guide  for

the Spalart-Allmaras based DES model and Equation . in the Theory Guide  for the realizable k-epsilon

based DES model.The DES length scale for the BSL / SST k-omega based DES model is defined by

, where

is a calibration constant used in the DES model and has a value of . and

is the maximum local grid spacing (

).

(in the Turbulence... category) is either the multiplier function

for Detached Eddy Simulation (DES)

with BSL, SST, or Transition SST (see DES with the BSL or SST k-ω Model and DES with the Transition SST

Model in the Theory Guide for details) or the function

for DES with Spalart-Allmaras or Realizable -

(see Theory Guide DES with the Spalart-Allmaras Model or DES with the Realizable k-ε Model, respectively).

Diameter

(in the Properties... category) is the diameter of particles, droplets, or bubbles of the secondary phase

selected in the Phase drop-down list. Its unit quantity is length.

(in the User Defined Scalars... category) is the diffusion coefficient for the

th user-defined scalar transport

equation. See the Fluent Customization Manual for details about defining user-defined scalars.

includes quantities related to the discrete phase model sources. See Modeling Discrete Phase (p. ) for

details about this model.

includes non-source quantities related to the discrete phase model. See Modeling Discrete Phase (p. )

for details about this model.

(in the Discrete Phase Variables... category) is the absorption coefficient for discrete-phase calculations

that involve radiation (  in Equation . in the Theory Guide ). Its unit quantity is length-inverse.

(in the Discrete Phase Variables... category) is the accretion rate calculated at a wall boundary:

(.)

where

is the mass flow rate of the particle stream, and

is the area of the wall face where

the particle strikes the boundary. This item will appear only if the optional erosion/accretion model

is enabled. See Monitoring Erosion/Accretion of Particles at Walls (p. ) for details. The unit

quantity for DPM Accretion is mass-flux.

(in the Discrete Phase Sources... category) is the exchange of mass from the discrete to the continuous

phase for the combustion law (Law ) and is proportional to the solid phase reaction rate.The burnout

exchange has units of mass-flow and is reported as the rate occurring in each cell. A unit cell depth is

used for 2D cases, and a reference cell depth of  radian is used for 2D axisymmetric cases.

(in the Discrete Phase Variables... category) is the time rate of particle-to-particle collisions per unit

volume. Its unit quantity is collision-rate.

(in the Discrete Phase Variables... category) is the total concentration of the particles in all phases in a

cell. Its unit quantity is density.

DPM Conc of <component>

(in the Discrete Phase Variables... category) is the mean concentration of <component> in the particles

within a cell, computed per phase.Therefore, when using DDPM, this quantity appears for each combination

of <component> and discrete particle phase (including the mixture phase). Its unit quantity is density.

(in the Discrete Phase Variables... category) is the mean particle density.This is computed as the mean

density of the particles in each cell and is computed per phase.Therefore, when using DDPM this quantity

is available for each discrete phase and the mixture phase. Its unit quantity is density.

(in the Discrete Phase Variables... category) is the mean particle diameter.This is computed as the mean

diameter of the discrete phase particles in each cell and is computed per phase.Therefore, when using

DDPM this quantity is available for each discrete phase and the mixture phase. Its unit quantity is length.

(in the Discrete Phase Variables... category) is the amount of radiation emitted by a discrete-phase particle

per unit volume. Its unit quantity is heat-generation-rate.

(in the Discrete Phase Sources... category) is the exchange of enthalpy (sensible enthalpy plus heat of

formation) from the discrete phase to the continuous phase.The exchange is positive when the particles

are a source of heat in the continuous phase.The unit quantity for DPM Enthalpy Source is power and

is reported as the rate of exchange occurring in each cell. A unit cell depth is used for 2D cases, and a ref-

erence cell depth of  radian is used for 2D axisymmetric cases.

(in the Discrete Phase Variables... category) is the erosion rate calculated at a wall boundary face using

Equation . in the Fluent Theory Guide based on the values entered in the Generic Erosion Model

Parameters dialog box (see Setting Particle Erosion and Accretion Parameters (p. )).This item will appear

only if the Erosion/Accretion option is selected in the Physical Models tab of the Discrete Phase Model

Dialog Box (p. ) and the Generic Model option is enabled in the DPM tab of the Wall Dialog Box (p. ).

See Monitoring Erosion/Accretion of Particles at Walls (p. ) for details.The unit quantity for DPM Erosion

Rate (Generic) is mass-flux.

(in the Discrete Phase Variables... category) is the Finnie erosion rate calculated using the Finnie formu-

lation. (See Accretion in the Fluent Theory Guide for background information about this model.) This item

will appear only if the Finnie option is enabled in the Physical Models tab of the Discrete Phase Model

Dialog Box (p. ). See Monitoring Erosion/Accretion of Particles at Walls (p. ) for details.The unit

quantity for DPM Erosion Rate (Finnie) is mass-flux.

(in the Discrete Phase Variables... category) is the McLaury erosion rate calculated using the McLaury

formulation. (See McLaury Erosion Model in the Fluent Theory Guide for background information about

this model.) This item will appear only if the McLaury erosion model is enabled in the Physical Models

tab of the Discrete Phase Model Dialog Box (p. ). See Monitoring Erosion/Accretion of Particles at

Walls (p. ) for details.The unit quantity for DPM Erosion Rate (McLaury) is mass-flux.

(in the Discrete Phase Variables... category) is the Oka erosion rate calculated using the Oka formulation.

(See Oka Erosion Model in the Fluent Theory Guide for background information about this model.) This item

will appear only if the Oka erosion model is enabled in the Physical Models tab of the Discrete Phase

Model Dialog Box (p. ). See Monitoring Erosion/Accretion of Particles at Walls (p. ) for details.The

unit quantity for DPM Erosion Rate (Oka) is mass-flux.

(in the Discrete Phase Variables... category) is the abrasive erosion rate calculated using the shear stress

formulation. See Modeling Erosion Rates in Dense Flows in the Fluent Theory Guide for background inform-

ation about this model. See Monitoring Erosion/Accretion of Particles at Walls (p. ) for details.The unit

quantity for DPM Erosion Rate (Wall Shear) is mass-flux.This quantity is available for dense flows for

which DPM erosion is enabled and with the disperse granular secondary phase.

(in the Discrete Phase Sources... category) is the exchange of mass, due to droplet-particle evaporation

or combusting-particle devolatilization, from the discrete phase to the evaporating or devolatilizing species.

If you are not using the non-premixed combustion model, the mass source for each individual species

(DPM species-n Source, below) is also available; for non-premixed combustion, only this sum is available.

The unit quantity for DPM Evaporation/Devolatilization is mass-flow and is reported as the rate of ex-

change occurring in each cell. A unit cell depth is used for 2D cases, and a reference cell depth of  radian

is used for 2D axisymmetric cases.

(in the Discrete Phase Variables... category) is the mean Granular Temperature for the discrete phase

particles within a cell. Its unit quantity is turbulent kinetic energy.This quantity is only available when

using a granular secondary phase in the Dense Discrete Phase Model.

(in the Discrete Phase Sources... category) is the total exchange of mass from the discrete phase to the

continuous phase.The mass exchange is positive when the particles are a source of mass in the continuous

phase. If you are not using the non-premixed combustion model, DPM Mass Source will be equal to the

sum of all species mass sources (DPM species-n Source, below); if you are using the non-premixed

combustion model, it will be equal to DPM Burnout plus DPM Evaporation/Devolatilization.The unit

quantity for DPM Mass Source is mass-flow and is reported as the rate of exchange occurring in each

cell. A unit cell depth is used for 2D cases, and a reference cell depth of  radian is used for 2D axisymmetric

cases.

DPM D20

(in the Discrete Phase Variables... category) is the surface mean diameter for the discrete phase particles

within a cell.This is computed per phase.Therefore, when using DDPM this quantity is available for each

discrete phase and the mixture phase. Its unit quantity is length. For the definition of the D20 diameter,

refer to Summary Reporting of Current Particles (p. ).

DPM D30

DPM D30

(in the Discrete Phase Variables... category) is the volume mean diameter for the discrete phase particles

discrete phase and the mixture phase. Its unit quantity is length. For the definition of the D30 diameter,

DPM D32

(in the Discrete Phase Variables... category) is the Sauter mean diameter for the discrete phase particles

discrete phase and the mixture phase. Its unit quantity is length. For the definition of the Sauter diameter,

DPM D43

(in the Discrete Phase Variables... category) is the mean diameter over volume (also called De Brouckere

mean diameter) for the discrete phase particles within a cell.This is computed per phase.Therefore, when

using DDPM this quantity is available for each discrete phase and the mixture phase. Its unit quantity is

length. For the definition of the De Brouckere diameter, refer to Summary Reporting of Current

(in the Discrete Phase Variables... category) is the number of particles per unit cell volume.This is com-

puted per phase.Therefore, when using DDPM this quantity is available for each discrete phase and the

mixture phase. Its unit quantity is volume-inverse.

(in the Discrete Phase Variables... category)

For steady particle tracking, this is the count of trajectories that entered the cell during the last DPM it-

eration.

For unsteady particle tracking, this is the count of particle parcels that entered the cell during the last

DPM iteration. Each parcel is weighted by the fraction of the fluid flow time step that it actually resides

in the cell.

This is computed per phase. Therefore, when using DDPM this quantity is available for each discrete

phase and the mixture phase.

For steady particle tracking, this is the time-constant number of particles that is represented by all tra-

jectories in the cell.

For unsteady particle tracking, this is the number of particles in all parcels that entered the cell during

the last DPM iteration, where each parcel is weighted by the fraction of the fluid flow time step that it

actually resides in the cell.

(in the Discrete Phase Variables... category) is the RMS particle diameter.This is computed as the RMS

particle diameter within each cell and is computed per phase.Therefore, when using DDPM, this quantity

is available for each discrete phase and the mixture phase. Its unit quantity is length.

(in the Discrete Phase Variables... category) is the RMS particle temperature.This is computed as the

RMS particle temperature within each cell and is computed per phase.Therefore, when using DDPM this

quantity is available for each discrete phase and the mixture phase. Its unit quantity is temperature.

(in the Discrete Phase Variables... category) are the RMS X,Y, and Z Velocity components of the discrete

phase.These are computed as the mean discrete phase RMS velocities and are computed per phase.

Therefore, when using DDPM these quantities are available for each discrete phase and the mixture phase.

Its unit quantity is velocity.

(in the Discrete Phase Variables... category) is the scattering coefficient for discrete-phase calculations

that involve radiation (

in Equation . in the Theory Guide ). Its unit quantity is length-inverse.

(in the Discrete Phase Sources... category) is the exchange of sensible enthalpy from the discrete phase

to the continuous phase.The exchange is positive when the particles are a source of heat in the continuous

phase. Its unit quantity is power and is reported as the rate of exchange occurring in each cell. A unit cell

depth is used for 2D cases, and a reference cell depth of  radian is used for 2D axisymmetric cases.

DPM species-n Source

(The name of the species will replace species-n  in DPM species-n Source.) These species can be

specified in the Set Injection Properties Dialog Box (p. ), and their descriptions can be found in Defining

Injection Properties (p. ).The unit quantity is mass-flow and is reported as the rate of exchange occurring

in each cell. A unit cell depth is used for 2D cases, and a reference cell depth of  radian is used for 2D

axisymmetric cases. Note that this variable will not be available if you are using the non-premixed combus-

tion model; use DPM Evaporation/Devolatilization instead.

(in the Discrete Phase Variables... category) is the mean particle specific heat.This is computed as the

mean specific heat of the particles within each cell and is computed per phase.Therefore, when using

DDPM this quantity is available for each discrete phase and the mixture phase. Its unit quantity is specific-

heat.

(in the Discrete Phase Sources... category) is the exchange of swirl momentum from the discrete phase

to the continuous phase.This value is positive when the particles are a source of momentum in the con-

tinuous phase.The unit quantity is force and is reported as the rate of exchange occurring in each cell. A

unit cell depth is used for 2D cases, and a reference cell depth of  radian is used for 2D axisymmetric

cases.

(in the Discrete Phase Variables... category) is the mean particle temperature.This is computed as the

mean temperature of the particles within each cell and is computed per phase.Therefore, when using

DDPM this quantity is available for each discrete phase and the mixture phase. Its unit quantity is temper-

ature.

ature.

(in the Discrete Phase Variables... category) is the volume fraction of the discrete phase.This is computed

as the mean discrete phase volume fraction within each cell and is computed per phase.Therefore, when

using DDPM this quantity is available for each discrete phase and the mixture phase.

(in the Discrete Phase Variables... category) is the magnitude of the wall force vector per unit area.

DPM Wall X,Y, Z Force

(in the Discrete Phase Variables... category) are the X,Y, and Z components of the DPM particle-wall

force.These are computed on all wall boundary conditions. For steady-state simulations, the reported

forces are the mean forces exerted by the particles per unit time. For transient simulations, the reported

forces are the accumulated particle-wall forces over the simulation time.

DPM X,Y, Z Momentum Source

(in the Discrete Phase Sources... category) are the exchange of -,

, and -direction momentum from

the discrete phase to the continuous phase.These values are positive when the particles are a source of

momentum in the continuous phase.The unit quantity is force and is reported as the rate of exchange

occurring in each cell. A unit cell depth is used for 2D cases, and a reference cell depth of  radian is used

for 2D axisymmetric cases.

(in the Discrete Phase Variables... category) are the X,Y, and Z Velocity components of the discrete phase.

These are computed as the mean discrete phase velocities and are computed per phase.Therefore, when

using DDPM these quantities are available for each discrete phase and the mixture phase. Its unit quantity

is velocity.

(in the Reactions… category) is the number of retained reactions in reduced mechanism.This variable

quantifies the size of the reduced mechanism at each cell or particle in the domain.

(in the Species... category) is the number of retained species in reduced mechanism.This variable quantifies

the size of the reduced mechanism at each cell or particle in the domain.

(in the Mesh... category) is the change of a cell volume.

(in the Pressure... category) is defined as

. Its unit quantity is pressure.

Echem Reaction Rate of Reaction-n

(in the Reactions... category) is the

th electrochemical reaction rate.This quantity is only available if the

electrochemical reaction model is enabled.

(in the Species... category) is the sum of the laminar and turbulent diffusion coefficients of a species into

the mixture:

(.)

(The name of the species will replace species-n  in Eff Diff Coef of species-n .) The unit

quantity is mass-diffusivity.

(in the Turbulence... category) is the ratio

, where

is the effective viscosity,

is the

specific heat, and

is the effective thermal conductivity.

(in the Properties... category) is the sum of the laminar and turbulent thermal conductivities,

, of the

fluid. A large thermal conductivity is associated with a good heat conductor and a small thermal conduct-

ivity with a poor heat conductor (good insulator). Its unit quantity is thermal-conductivity.

(in the Turbulence... category) is the sum of the laminar and turbulent viscosities of the fluid.Viscosity,

, is defined by the ratio of shear stress to the rate of shear. Its unit quantity is viscosity.

(in the Potential... category) is the electric potential  used in Equation . in the Fluent Theory Guide.

(in the Properties... category) is the electric conductivity  used in Equation . in the Fluent Theory

Guide.

(in the Potential... category) is either the electrode potential (

in the Butler-Volmer Equation .

in the Fluent Theory Guide) for walls with Faradaic reaction, or the wall potential after considering

the contact resistance effect for walls without Faradaic reaction.

Enthalpy

(in the Temperature... category) is defined differently for compressible and incompressible flows, and

depending on the solver and models in use.

For compressible flows,

(.)

and for incompressible flows,

(.)

where

and

are, respectively, the mass fraction and enthalpy of species . (See Enthalpy of

species-n , below). For the pressure-based solver, the second term on the right-hand side of

Equation . (p. ) is included only if the pressure work term is included in the energy equation

(see Inclusion of Pressure Work and Kinetic Energy Terms in the Theory Guide). For multiphase

models, this value corresponds to the selected phase in the Phase drop-down list. For all reacting

flow models, the Enthalpy plots consist of the thermal (or sensible) plus chemical energy. The unit

quantity for Enthalpy is specific-energy.

In the case of the inert model (Using the Non-Premixed Model with the Inert Model in the Theory

Guide ), the enthalpy in a cell is split into the contributions from the inert and the reacting fractions

of the gas phase species in the cell. The cell enthalpy is partitioned as

(.)

where  is the fraction of inert species in the cell. The quantity

is the enthalpy of the inert

species at the cell temperature, similarly

is the enthalpy of the active species at the cell tem-

perature. It is assumed that the cell temperature is common to both inert and active species, so

,

and the cell temperature are chosen so that Equation . (p. ) is satisfied.

Enthalpy of species-n

(in the Species... category) is defined differently depending on the solver and models options in use.The

quantity:

(.)

where

is the formation enthalpy of species  at the reference temperature

, is

reported only for non-adiabatic PDF cases, or if the density-based solver is selected. The quantity:

(.)

where

, is reported in all other cases. The unit quantity for Enthalpy of species-

n  is specific-energy.

Entropy

(in the Temperature... category) is a thermodynamic property defined by the equation

(.)

(.)

the entropy is computed using the equation

(.)

The unit quantity for entropy is specific-heat.

Important

Note that for the real gas models the entropy is computed accordingly by the appropriate

equation of state formulation.

(in the Adaption... category) is the value that presently resides in the temporary space reserved for cell

variables (that is, the last value that you displayed or computed).

(in the Mesh... category) is the magnitude of the face area vector for noninternal faces (that is, faces that

only have c0 and no c1).The values are stored on the face itself and used when required.This variable is

intended only for zone surfaces and not for other surfaces created for postprocessing.

(in the Mesh... category) is a parameter that is equal to one in cells that are adjacent to left-handed faces,

and zero elsewhere. It can be used to locate mesh problems.

(in the Potential... category) is the electric current density produced by the electrochemical reaction at

Faradaic interfaces (Equation . in the Fluent Theory Guide). Faradaic current density is positive if electric

current flows from the electrode zone to the electrolyte zone, and negative if the electric current flows in

the reverse direction.

(in the Potential... category) is the energy source term due to the electrochemical reaction at Faradaic

interfaces (Equation . in the Fluent Theory Guide).

(in the Eulerian Wall Film... category) is the Courant number of the wall film.

(in the Eulerian Wall Film... category) is the value of film wet area fraction as defined in Equation .

in the Fluent Theory Guide.In reporting, the face integral of this variable gives the area covered by the film.

This item is available when Solve Momentum is enabled in the Eulerian Wall Film dialog box.

(in the Eulerian Wall Film... category) is the additional energy of discrete particles being absorbed into

the wall film.

(in the Eulerian Wall Film... category) is the additional mass of discrete particles being absorbed into the

wall film.

(in the Eulerian Wall Film... category) is the x-component of any additional momentum of discrete particles

being absorbed into the wall film.

(in the Eulerian Wall Film... category) is the y-component of any additional momentum of discrete particles

(in the Eulerian Wall Film... category) is the z-component of any additional momentum of discrete particles

(in the Eulerian Wall Film... category) is the effective pressure of the wall film.

Film Mass

(in the Eulerian Wall Film... category) is the mass of the wall film.

(in the Eulerian Wall Film... category) is the cumulative mass of film outflow.

(in the Eulerian Wall Film... category) is the passive scalar for the wall film scalar equation.

(in the Eulerian Wall Film... category) is the phase change rate, with positive value as the condensation

rate and negative value as the vaporization rate.This item is available when Phase Change is enabled.

Film Secondary Phase Collection Coef

(in the Eulerian Wall Film... category) is the coefficient of secondary phase collection.This item is available

when Phase Accretion is enabled.

(in the Eulerian Wall Film... category) is the mass of secondary phase collection.This item is available

(in the Eulerian Wall Film... category) is the diameter of separated wall film droplet.This item is available

when Edge Separation is enabled.

(in the Eulerian Wall Film... category) is the diameter of stripped wall film droplets.

(in the Eulerian Wall Film... category) is the cumulative mass of stripped wall film.

(in the Eulerian Wall Film... category) is the surface temperature of the wall film.

(in the Eulerian Wall Film... category) is the magnitude of the surface velocity of the wall film.

(in the Eulerian Wall Film... category) is the x-component of the surface velocity of the wall film.

(in the Eulerian Wall Film... category) is the y-component of the surface velocity of the wall film.

(in the Eulerian Wall Film... category) is the z-component of the surface velocity of the wall film.

(in the Eulerian Wall Film... category) is the temperature of the wall film.

(in the Eulerian Wall Film... category) is the thickness of the wall film.

(in the Eulerian Wall Film... category) is the magnitude of the velocity of the wall film.

(in the Eulerian Wall Film... category) is the Weber number of the wall film.

Film X-Momentum Source

(in the Eulerian Wall Film... category) is the x-component of any additional momentum being absorbed

into the wall film.

Film Y-Momentum Source

(in the Eulerian Wall Film... category) is the y-component of any additional momentum being absorbed

(in the Eulerian Wall Film... category) is the x-component of the velocity of the wall film.

(in the Eulerian Wall Film... category) is the y-component of the velocity of the wall film.

(in the Eulerian Wall Film... category) is the z-component of the velocity of the wall film.

Fine Scale Mass Fraction of species-n

(in the Species... category) is the term

in Equation . in the Theory Guide .

(in the Temperature... category) is the temperature of the fine scales, which is calculated from the enthalpy

when the reaction proceeds over the time scale (

in Equation . in the Theory Guide ), governed by

the Kinetic rates of Equation . in the Theory Guide . Its unit quantity is temperature.

Fine Scale Transfer Rate

(in the Species... category) is the transfer rate of the fine scales, which is equal to the inverse of the time

scale (

Fine Scale Volume Fraction

(in the Species... category) is a function of the fine scale volume fraction (

scale (

Guide ).The quantity is subtracted from unity to make it easier to interpret.

(in the Eulerian Wall Film... category) is the cumulative mass of separated wall film.

(in the Premixed Combustion... category) is the rate of production of species-n due to forward reactions

for scalar  in kg/m3/s (

in Equation . in the Fluent Theory Guide). (The name of the PDF scalar

will replace PDF scalar-n in Forward Reaction Rate of PDF scalar-n.)

Fvar Prod

(in the Pdf... category) is the production term in the mixture fraction variance equation solved in the non-

premixed combustion model (that is, the last two terms in Equation . in the Theory Guide ).

Fvar2 Prod

(in the Pdf... category) is the production term in the secondary mixture fraction variance equation solved

in the non-premixed combustion model. See Equation . in the Theory Guide .

(in the Properties... category) is the gas constant of the fluid. Its unit quantity is specific-heat.

(in the Turbulence... category) is used in the roughness correlation of the Transition SST model. See

Equation . in the Theory Guide.

(in the Properties... category) is equivalent to the diffusion coefficient in Equation . in the Theory

Guide . For more information, see Granular Temperature in the Theory Guide . Its unit quantity is kg/m-s.

includes quantities for reporting the solids pressure for each granular phase (

Theory Guide ). See Solids Pressure in the Theory Guide for details. Its unit quantity is pressure. For mul-

tiphase models, this value corresponds to the selected phase in the Phase drop-down list.

includes quantities for reporting the granular temperature for each granular phase (

in the Theory Guide ). See Granular Temperature in the Theory Guide for details. Its unit quantity is

.

For multiphase models, this value corresponds to the selected phase in the Phase drop-down list.

HCN Density

(in the NOx... category) is the mass per unit volume of HCN.The unit quantity is density.The HCN Density

will appear only if you are modeling fuel NOx. See Fuel NOx Formation in the Theory Guide for details.

(in the Phase Interaction... category) is the heat added or removed due to heterogeneous chemical reac-

tions. For exothermic reactions the Heat of Heterogeneous Reaction is reported as a positive quantity,

while for endothermic reactions it will be a negative quantity. If you have more than one heterogeneous

reaction defined in your case, the Heat of Heterogeneous Reaction reported is the sum of the heat for

all heterogeneous reactions.The unit quantity of Heat of Heterogeneous Reaction is Watt.

(in the Reactions... category) is the heat added or removed due to chemical reactions.The quantity reported

by Fluent is the volumetric heat of reaction, as defined in Equation . in the Theory Guide  multiplied

by the cell volume. For exothermic reactions, the heat of reaction is reported as a positive quantity, while

for endothermic reactions it is reported as a negative quantity. If you have more than one reaction defined

in your case, the Heat of Reaction reported is the sum of the heat for all reactions.The unit of measurement

for the heat of reaction is Watts.The Heat of Reaction is not available for the non-premixed and partially-

premixed models.

(in the Pdf... category) is the rate of heat generated due to chemical reaction (J/m3/s) as defined in Equa-

tion . in the Fluent Theory Guide.

Helicity

(in the Velocity... category) is defined by the dot product of vorticity and the velocity vector.

(.)

Vorticity is a measure of the rotation of a fluid element as it moves in the flow field.

(in the Radiation... category) is the total radiation energy,

, that arrives at a location per unit time and

per unit area:

(.)

where  is the radiation intensity and

is the solid angle.

is the quantity that the P- radiation

model computes. For the DO radiation model, the incident radiation is computed over a finite

number of discrete solid angles, each associated with a vector direction. For the MC model, the ra-

diation intensity is computed by tallying the distance travelled by photons in each cell. The unit

quantity for Incident Radiation is heat-flux.

Incident Radiation (Band n)

(in the Radiation... category) is the radiation energy contained in the wavelength band

for the non-

gray P-, DO, or MC radiation models. Its unit quantity is heat-flux.

(in the Mesh... category) is a metric for measuring the quality of the intersection between interface zones

for non-conformal interfaces. It is calculated on each element of the interface zone and ranges from  to

, where  means no intersection, and  means full intersection.

(in the Turbulence... category) is a measure of the probability that a given point is located inside a turbulent

region. Upstream of transition the intermittency is zero. Once the transition occurs, the intermittency is

ramped up to one until the fully turbulent boundary layer regime is achieved.

(in the Turbulence... category) is used in the coupling of the Transition model and the SST Transport

equations (see Coupling the Transition Model and SST Transport Equations in the Theory Guide for details).

(in the Temperature... category) is the summation of the kinetic and potential energies of the molecules

of the substance per unit volume (and excludes chemical and nuclear energies). Internal Energy is defined

as

. Its unit quantity is specific-energy.

(in the Acoustics... category) is the acoustic power for turbulent axisymmetric jets (see Equation . in

the Theory Guide ). It is available only when the Broadband Noise Sources acoustics model is being used.

(in the Acoustics... category) is the acoustic power for turbulent axisymmetric jets, reported in dB (see

Equation . in the Theory Guide). It is available only when the Broadband Noise Sources acoustics

model is being used.

(in the Potential... category) is the energy source term due to the Joule heating (Equation . in the

(in the Reactions... category) is given by the following expression (see Equation . in the Theory Guide

for definitions of the variables shown here):

(.)

The reported value is independent of any particular species, and has units of kmol/

s.

To find the rate of production/destruction for a given species  due to reaction , multiply the re-

ported reaction rate for reaction  by the term

, where

is the molecular weight of

species , and

and

are the stoichiometric coefficients of species  in reaction .

For particle reactions it is the global rate of the particle reaction n expressed in kmol/s/m3. This is

computed as

where

is the rate of particle species depletion (or generation) given by Equation . in the

Theory Guide ,

is the particle species molecular weight, and

(in the Turbulence... category) is a postprocessing quantity used for visual inspection of turbulence

structures.

(in the Species... category) is the laminar diffusion coefficient of a species into the mixture,

. Its unit

(in the Premixed Combustion... category) is the propagation speed of laminar premixed flames (

in

Equation . in the Theory Guide ). Its unit quantity is velocity.

Laminar Kinetic Energy (kl)

(in the Turbulence...category) is a measure of the “laminar” streamwise fluctuations present in the pre-

transitional region of the boundary layer subjected to free-stream turbulence. A transport equation of kl

is considered by the k-kl-omega transition model.

(in the Phase Interaction... category) is the latent heat for the n th mass transfer mechanism that you

defined.

LEE Self-Noise X-Source, LEE Self-Noise Y-Source, LEE Self-Noise Z-Source

(in the Acoustics... category) are the self-noise source terms in the linearized Euler equation for the

acoustic velocity component (see Equation . in the Theory Guide ).They are available only when the

Broadband Noise Sources acoustics model is being used.

LEE Shear-Noise X-Source, LEE Shear-Noise Y-Source, LEE Shear-Noise Z-Source

(in the Acoustics... category) are the shear-noise source terms in the linearized Euler equation for the

LEE Total Noise X-Source, LEE Total Noise Y-Source, LEE Total Noise Z-Source

(in the Acoustics... category) are the total noise source terms in the linearized Euler equation for the

acoustic velocity component (see Equation . in the Theory Guide ).The total noise source term is the

sum of the self-noise and shear-noise source terms.They are available only when the Broadband Noise

Sources acoustics model is being used.

(in the Turbulence... category) is the eddy viscosity that is determined by the local algebraic sub-grid

scale model in an embedded LES zone, which actually affects the momentum transport equations (see

Embedded Large Eddy Simulation (ELES) in the Theory Guide ). Its unit quantity is viscosity.

(in the Acoustics... category) is the self-noise source term in the linearized Lilley’s equation (see Equa-

tion . in the Theory Guide ), available only when the Broadband Noise Sources acoustics model is

being used.

(in the Acoustics... category) is the shear-noise source term in the linearized Lilley’s equation (see Equa-

(in the Acoustics... category) is the total noise source term in the linearized Lilley’s equation (see Equa-

tion . in the Theory Guide ).The total noise source term is the sum of the self-noise and shear-noise

source terms, available only when the Broadband Noise Sources acoustics model is being used.

(in the Solidification/Melting... category) is the liquid fraction  computed by the solidification/melting

model:

(.)

(.)

(.)

(in the Sensitivities... category) provides a convenience function that plots

of the magnitude, in

view of the large range of values possible for the shape sensitivity magnitude.This allows the importance

of the surfaces in a domain to be ranked more easily based on how they affect the observation of interest

when they are reshaped.

(in the Lump Detection... category) is a measure of the non-sphericity of the liquid lump according to the

surface-radius orthogonality method.

radius standard deviation method.

(in the Lump Detection... category) is a volume-weighted average of the lump density.

(in the Lump Detection... category) is the diameter of a volume-equivalent sphere.

(in the Lump Detection... category) is the average specific enthalpy of the lump.This quantity is available

only when the energy equation is enabled.

Lump ID

(in the Lump Detection... category) is a unique integer value for every contiguous portion of liquid. One

ID is assigned to the liquid core, and other IDs are assigned to each detached lump.

(in the Lump Detection... category) is the average pressure of the lump.This quantity is available only

when the energy equation is enabled.

(in the Lump Detection... category) is the average temperature of the lump.This quantity is available only

(in the Lump Detection... category) are the X,Y, and Z coordinates of the center of gravity of the liquid

lump.

(in the Lump Detection... category) are the X,Y, and Z components of the liquid lump velocity vector.

(in the Velocity... category) is the ratio of velocity and speed of sound.

Magnitude of Sensitivity to Body Forces (Cell Values)

(in the Sensitivities... category) is the magnitude of the adjoint velocity primitive field.This field can be

interpreted as the magnitude of the sensitivity of the observable to body force per unit volume. It can be

used to identify regions in the domain where small changes to the momentum balance in the flow can

have a large or small effect on the observable.This field is often observed to be large, for example, upstream

of a body for which drag sensitivity is of interest, with the field diminishing in the upstream direction.This

indicates the interference effect for an object positioned at various locations upstream of the object of

interest.

(in the Mesh... category) is a parameter that is equal to one in cells that are identified as invalid or poor,

as well as cells that are adjacent to the face of an invalid or poor cell, and zero elsewhere. It can be used

to mark and/or display invalid and poor elements.

Mass fraction of HCN, Mass fraction of NH3, Mass fraction of NO, Mass fraction of N2O

(in the NOx... category) are the mass of HCN, the mass of

, the mass of NO, and the mass of N2O per

unit mass of the mixture (for example, kg of HCN in  kg of the mixture).The Mass fraction of HCN and

the Mass fraction of NH3 will appear only if you are modeling fuel NOx. See Fuel NOx Formation in the

Theory Guide  for details.

Mass fraction of nuclei

(in the Soot... category) is the number of particles per unit mass of the mixture (in units of particles

/kg) The Mass fraction of nuclei will appear only if you use the two-step soot model. See Soot

Formation (p. ) for details.

Mass fraction of soot

(in the Soot... category) is the mass of soot per unit mass of the mixture (for example, kg of soot in  kg

of the mixture). See Soot Formation (p. ) for details.

(in the Species... category) is the mass of a species per unit mass of the mixture (for example, kg of species

in  kg of the mixture).

(in the Phase Interaction... category) is the mass transfer rate for the n th mass transfer mechanism that

you defined.

Mean n

(in the Steady Statistics... or Unsteady Statistics... category) is the iteration- or time-averaged value of

a solution variable n (for example, Static Pressure). See Performing Steady-State Calculations (p. ) and

Postprocessing for Time-Dependent Problems (p. ) for details.

Mean- cff_n

a custom field function cff_n (for example, uns-custom-function-). See Performing Steady-State Calcula-

tions (p. ) and Postprocessing for Time-Dependent Problems (p. ) for details.

Mean DPM n

a discrete phase variable n (for example, Volume Fraction). See Performing Steady-State Calculations (p. )

and Postprocessing for Time-Dependent Problems (p. ) for details.

(in the Mesh... category) is the normalized (dimensionless) coordinate that follows the flow path from inlet

to outlet. Its value varies from  to .

Mesh...

includes variables related to the mesh.

Mesh X-Velocity, Mesh Y-Velocity, Mesh Z-Velocity

(in the Velocity... category) are the vector components of the mesh velocity for moving-mesh problems

(rotating or multiple reference frames, mixing planes, or sliding meshes). Its unit quantity is velocity.

(in the Pdf... category) is the variance of the mixture fraction solved for in the non-premixed combustion

model.This is the second conservation equation (along with the mixture fraction equation) that the non-

premixed combustion model solves. (See Definition of the Mixture Fraction in the Theory Guide .)

(in the Turbulence... category) is the transported quantity  that is solved for in the Spalart-Allmaras tur-

bulence model and in DES with the Spalart-Allmaras model (see Equation . in the Theory Guide ).The

turbulent viscosity,

, is computed directly from this quantity using the relationship given by Equation .

in the Theory Guide . Its unit quantity is viscosity.

(in the Species... category) is the moles per unit volume of a species. Its unit quantity is concentration.

(in the Species... category) is the number of moles of a species in one mole of the mixture.

Mole fraction of HCN, Mole fraction of NH3, Mole fraction of NO, Mole fraction of N2O

(in the NOx... category) are the number of moles of HCN,

, NO, and N2O in one mole of the mixture.

The Mole fraction of HCN and the Mole fraction of NH3 will appear only if you are modeling fuel NOx.

See Fuel NOx Formation in the Theory Guide  for details.

Mole fraction of soot

(in the Soot... category) is the number of moles of soot in one mole of the mixture.

(in the Properties... category) is the ratio

.

(in the Properties... category) is the laminar viscosity of the fluid.Viscosity,

, is defined by the ratio of

shear stress to the rate of shear. Its unit quantity is viscosity. For multiphase models, this value corresponds

to the selected phase in the Phase drop-down list. For a granular phase, the molecular viscosity is multiplied

by the granular volume fraction.

Momentum Thickness Re (

)

(in the Turbulence... category) is based on the momentum thickness of the boundary layer.The SST

transition model is considering a nonlocal empirical correlation for the value of

in the free-stream,

based on turbulence intensity, pressure gradient, and so on, and a transport equation to allow the free-

stream value to diffuse into the boundary layer.

NH3 Density, NO Density, N2O Density

(in the NOx... category) are the mass per unit volume of NH3, NO, and N2O.The unit quantity for each is

density.The NH3 Density will appear only if you are modeling fuel NOx. See Fuel NOx Formation in the

Non-Equilibrium Thermal Model Source

(in the Temperature... category) is the scaled value of thermal conductivity for the fluid zone (

) or for

the overlapping solid zone (

), where  is the porosity,

), and

is the solid medium thermal conductivity.These terms

can be seen in Equation . (p. ) and Equation . (p. ).

), and

See Non-Equilibrium Thermal Model Equations (p. ) and Non-Equilibrium Thermal Model (p. )

for details about the non-equilibrium thermal model.

(in the Sensitivities... category) shows the normal component of the optimal displacement computed

from the adjoint solution.This field is defined only for portions of walls lying within the control-volume

specified for morphing.The size of the optimal displacement is determined by the scale factor that is

chosen for the morphing. A positive value of displacement indicates that the surface will be displaced into

the flow domain, whereas a negative value of displacement corresponds to wall movement outwards from

the flow domain.This field eliminates the component of the optimal displacement vector that lies in the

plane of the wall.

(in the Sensitivities... category) shows the normal component of the shape sensitivity. A positive value

indicates an orientation directed into the domain, while a negative value indicates that the shape sensitivity

is oriented outwards from the domain.This field eliminates the component of the vector shape sensitivity

field that lies in the plane of the wall.

Normalized Concentration of Nuclei

(in the Soot... category) is the normalized soot particle number density.

(in the Soot... category) is the normalized soot aggregate moments.This quantity is available only with

the Method of Moments model.

Normalized soot moments

(in the Soot... category) are the normalized soot moments.This quantity is available only with the Method

of Moments model.

NOx...

contains quantities related to the NOx model. See NOx Formation (p. ) for details about this model.

(in the Mesh... category) is a measure of the quality of a mesh, and is computed for each cell using the

vectors from the cell centroid to each of its faces, the area vectors of the cell's faces, and the vectors from

the cell centroid to the centroids of each of the adjacent cells (see Equation . (p. ) and Equa-

tion . (p. )).The worst cells will have an Orthogonal Quality closer to , with better cells closer to .

(in the Cell Info... category) is an integer value indicating the overset cell type. Each cell can have one of

the following values:

Integer Function

Value

Cell Type

donor

solve

receptor

–

orphan

–

dead

(in the Cell Info... category) shows the number of donor cells a receptor cell has for data interpolation. A

value of zero indicates that the cell is not a receptor, or that the receptor cell is an orphan cell.

(in the Cell Info... category) shows the number of receptor cells referencing a donor cell. A value of zero

indicates that the cell is not a donor cell.

Primary Particle Diameter

(in the Soot... category) is a soot primary particle diameter within soot aggregates.This quantity is available

only with the Method of Moments model.

Partition Boundary Cell Distance

(in the Mesh... category) is the smallest number of cells that must be traversed to reach the nearest partition

(interface) boundary.

(in the Cell Info... category) is the number of adjacent partitions (that is, those that share at least one

partition boundary face (interface)). It gives a measure of the number of messages that will have to be

generated for parallel processing.

Pdf...

contains quantities related to the non-premixed combustion model, which is described in Modeling Non-

Premixed Combustion (p. ).

is the adiabatic enthalpy corresponding to the cell value of mixture fraction. For single mixture fraction

cases it is given by the following equation:

(.)

and for cases involving a secondary stream it is given by the following equation:

(.)

where

= mixture fraction

= secondary mixture fraction

= total enthalpy of the fuel stream

= total enthalpy of the secondary stream

= total enthalpy of the oxidizer stream

For adiabatic cases the PDF Table Adiabatic Enthalpy is equal to the value of Enthalpy. The unit

of measurement is specific-energy.

is given by the following equation:

(.)

if the cell enthalpy is less than the adiabatic enthalpy, and by the following equation:

(.)

if the cell enthalpy is higher than adiabatic

where

= total enthalpy

= the PDF Table Adiabatic Enthalpy

(.)

where

= the minimum Enthalpy defined in the PDF table

= the maximum Enthalpy defined in the PDF table

The PDF Table Heat Loss/Gain is dimensionless and ranges in value from -, when

is equal to

, to +, when

is equal to

. If H is equal to the adiabatic enthalpy it will be .

Phases...

contains quantities for reporting the volume fraction of each phase. See Modeling Multiphase Flows (p. )

(in the Mesh... category) is the normalized (dimensionless) coordinate in the circumferential (pitchwise)

direction. Its value varies from  to .

Porous Deposition Rate of species-n

(in the Species... category) is the amount of a surface species that is deposited on porous zones. Its unit

quantity is mass-flux.

(in the Velocity... category) is the reference velocity used in the coupled solver’s preconditioning  algorithm.

See Preconditioning in the Theory Guide  for details.

contains quantities related to the premixed combustion model, which is described in Modeling Premixed

Combustion (p. ).

includes quantities related to a normal force per unit area (the impact of the gas molecules on the surfaces

of a control volume).

(in the Pressure... category) is a dimensionless parameter defined by the equation

(.)

and

is the reference dynamic pressure defined by

. The reference pressure, density,

and velocity are defined in the Reference Values Task Page (p. ).

Pressure Spectrum Im n

(in the Acoustics... category) is the imaginary part of the complex Fourier amplitudes for Fourier mode n,

as calculated by the Acoustic Sources FFT Dialog Box (p. ). See FFT of Acoustic Sources: Band Analysis

and Export of Surface Pressure Spectra (p. ) for details.

Pressure Spectrum Re n

(in the Acoustics... category) is the real part of the complex Fourier amplitudes for Fourier mode n, as

calculated by the Acoustic Sources FFT Dialog Box (p. ). See FFT of Acoustic Sources: Band Analysis and

Export of Surface Pressure Spectra (p. ) for details.

(in the Premixed Combustion... category) is the source term in the progress variable transport equation

(

(in the Turbulence... category) is the rate of production of turbulence kinetic energy (times density). Its

unit quantity is turb-kinetic-energy-production. For multiphase models, this value corresponds to the

selected phase in the Phase drop-down list.

(in the Turbulence... category) is the production of laminar kinetic energy used in the -

transition

model. See Transport Equations for the k-kl-ω Model in the Theory Guide for more details (Equation . ).

(in the Premixed Combustion... category) is a normalized mass fraction of the combustion products (

)

or unburnt mixture products (

), as defined by Equation . in the Theory Guide .

(in the Premixed Combustion... category) is the variance of the reaction progress variable  that is solved

in the partially-premixed combustion model.

includes material property quantities for fluids and solids.

Rate of Coagulation

(in the Soot... category) is the rate of the coagulation of soot particles.

Rate of NO

(in the NOx... category) is the overall rate of formation of NO due to all active NO formation pathways (for

example, thermal, prompt, and so on).

Rate of Nucleation

(in the Soot... category) is the rate of nucleation of the soot particles.

Rate of Nuclei

(in the Soot... category) is the overall rate of formation of nuclei.

Rate of N2OPath NO

(in the NOx... category) is the rate of formation of NO due to the N2O pathway only (only available when

N2O pathway is active).

Rate of Oxidation

(in the Soot... category) is the rate of oxidation of the soot particles.

Rate of Prompt NO

(in the NOx... category) is the rate of formation of NO due to the prompt pathway only (only available

when prompt pathway is active).

Rate of Reburn NO

(in the NOx... category) is the rate of formation of NO due to the reburn pathway only (only available when

reburn pathway is active).

Rate of SNCR NO

(in the NOx... category) is the rate of formation of NO due to the SNCR pathway only (only available when

SNCR pathway is active).

(in the Soot... category) is the overall rate of formation of soot mass.

Rate of Soot Mass Nucleation

(in the Soot... category) is the overall rate of soot nucleation.

Rate of Surface Growth

(in the Soot... category) is the rate of the soot particle surface growth due to reactions at soot particle

surface.

Rate of Thermal NO

(in the NOx... category) is the rate of formation of NO due to the thermal pathway only (only available

when thermal pathway is active).

Rate of Fuel NO

(in the NOx... category) is the rate of formation of NO due to the fuel pathway only (only available when

fuel pathway is active).

Rate of USER NO

(in the NOx... category) is the rate of formation of NO due to user defined rates only (only available when

user-defined function rates are added).

(in the Mesh... category) is the length of the radius vector in the polar coordinate system.The radius vector

is defined by a line segment between the node and the axis of rotation.You can define the rotational axis

in the Fluid Dialog Box (p. ). (See also Velocity Reporting Options (p. ).) The unit quantity for Radial

Coordinate is length.

Radial Pull Velocity

(in the Solidification/Melting... category) is the radial-direction component of the pull velocity for the

(in the Velocity... category) is the component of velocity in the radial direction. (See Velocity Reporting

Options (p. ) for details.) The unit quantity for Radial Velocity is velocity. For multiphase models, this

value corresponds to the selected phase in the Phase drop-down list.

Radial-Wall Shear Stress

(in the Wall Fluxes... category) is the radial component of the force acting tangential to the surface due

to friction. Its unit quantity is pressure.

includes quantities related to radiation heat transfer. See Modeling Radiation (p. ) for details about the

radiation models available in ANSYS Fluent.

(in the Wall Fluxes... category) is the rate of radiation heat transfer through the control surface. It is calcu-

lated by the solver according to the specified radiation model. Heat flux out of the domain is negative,

and heat flux into the domain is positive.The unit quantity for Radiation Heat Flux is heat-flux.

Radiation Intensity.Normalized Std Deviation

(in the Radiation... category) is the statistical standard deviation for the spherical mean radiation intensity.

(in the Radiation... category) is the quantity

, defined by

(.)

where  is the Incident Radiation. The unit quantity for Radiation Temperature is temperature.

Rate of Reaction-n

(in the Reactions... category) is the effective rate of progress of

th reaction. For the finite-rate model, the

value is the same as the Kinetic Rate of Reaction-n. For the eddy-dissipation model, the value is equivalent

to the Turbulent Rate of Reaction-n. For the finite-rate/eddy-dissipation model, it is the lesser of the two.

where

where

includes quantities related to finite-rate reactions. See Modeling Species Transport and Finite-Rate

Chemistry (p. ) for information about modeling finite-rate reactions.

Reactor Net Mass Fraction of Species-n

(in the Species... category) is the mass of a species per unit mass of the mixture in the reactor network.

(in the Species... category) is the computed temperature of the reactor network.

(in the Species... category) a unique identifier associated with each reactor network.

of the fluid temperature  divided by the critical temper-

ature

.The reduced temperature

is available only with the Angier-Redlich-Kwong real gas model.

of the fluid pressure  divided by the critical pressure

.

The reduced pressure

Reflected Radiation Flux (Band-n)

(in the Wall Fluxes... category) is the amount of radiative heat flux reflected by a semi-transparent wall

Reflected Visible Solar Flux, Reflected IR Solar Flux

(in the Wall Fluxes... category) is the amount of solar heat flux reflected by a semi-transparent wall or

(in the Radiation... category) is a nondimensional parameter defined as the ratio of the speed of light in

a vacuum to that in a material. See Specular Semi-Transparent Walls in the Theory Guide  for details.

Relative Axial Velocity

(in the Velocity... category) is the axial-direction component of the velocity relative to the reference frame

motion. See Velocity Reporting Options (p. ) for details.The unit quantity for Relative Axial Velocity

(in the Species... category) is the ratio of the partial pressure of the water vapor actually present in an air-

water mixture to the saturation pressure of water vapor at the mixture temperature. ANSYS Fluent computes

the saturation pressure, , from the following equation  [] (p. ):

(.)

where

= . MPa

= . K

=

=

=

=

=

=

=

=

= .

= . K

Relative Mach Number

(in the Velocity... category) is the nondimensional ratio of the relative velocity and speed of sound.

Relative Radial Velocity

(in the Velocity... category) is the radial-direction component of the velocity relative to the reference frame

motion. (See Velocity Reporting Options (p. ) for details.) The unit quantity for Relative Radial Velocity

Relative Swirl Velocity

(in the Velocity... category) is the tangential-direction component of the velocity relative to the reference

frame motion, in an axisymmetric swirling flow. (See Velocity Reporting Options (p. ) for details.) The

unit quantity for Relative Swirl Velocity is velocity.

frame motion. (See Velocity Reporting Options (p. ) for details.) The unit quantity for Relative Tangential

Velocity is velocity.

(in the Pressure... category) is the stagnation pressure computed using relative velocities instead of absolute

velocities; that is, for incompressible flows the dynamic pressure would be computed using the relative

velocities. (See Velocity Reporting Options (p. ) for more information about relative velocities.) The unit

quantity for Relative Total Pressure is pressure.

Relative Total Temperature

(in the Temperature... category) is the stagnation temperature computed using relative velocities instead

of absolute velocities. (See Velocity Reporting Options (p. ) for more information about relative velocities.)

The unit quantity for Relative Total Temperature is temperature.

(in the Velocity... category) is similar to the Velocity Angle except that it uses the relative tangential ve-

locity, and is defined as

(.)

Its unit quantity is angle.

Relative Velocity Magnitude

(in the Velocity... category) is the magnitude of the relative velocity vector instead of the absolute velocity

vector.The relative velocity (

) is the difference between the absolute velocity ( ) and the mesh velocity.

For simple rotation, the relative velocity is defined as

(.)

where

is the angular velocity of a moving reference frame about the origin and  is the position

vector. (See Velocity Reporting Options (p. ) for details.) The unit quantity for Relative Velocity

Magnitude is velocity.

Relative X Velocity, Relative Y Velocity, Relative Z Velocity

(in the Velocity... category) are the -,

, and -direction components of the velocity relative to the ref-

erence frame motion. (See Velocity Reporting Options (p. ) for details.) The unit quantity for these variables

contains different quantities for the pressure-based and density-based solvers:

In the density-based solvers, this category includes the corrections to the primitive variables pressure,

velocity, temperature, and species, as well as the time rate of change of the corrections to these

primitive variables for the current iteration (that is, residuals). Corrections are the changes in the

variables between the current and previous iterations and residuals are computed by dividing a

cell’s correction by its physical time step. The total residual for each variable is the summation of

the Euler, viscous, and dissipation contributions. The dissipation components are the vector com-

ponents of the flux-like, face-based dissipation operator.

In the pressure-based solver, only the Mass Imbalance in each cell is reported (unless you have

requested others, as described in Postprocessing Residual Values (p. )). At convergence, this

quantity should be small compared to the average mass flow rate.

(in the Premixed Combustion... category) is the rate of consumption of species-n due to reverse reac-

tions for scalar  in kg/m3/s (

in Equation . in the Fluent Theory Guide). (The name of the PDF

scalar will replace PDF scalar-n in Reverse Reaction Rate of PDF scalar-n.)

RMS (species-n) Mass Fraction

(in the Species... category) is the root mean square value of the mass of a species per unit mass of the

mixture.

RMSE n

(in the Steady Statistics... or Unsteady Statistics... category) is the root mean squared error value of a

solution variable n (for example, Static Pressure). See Performing Steady-State Calculations (p. ) and

RMSE- cff_n

custom field function cff_n (for example, uns-custom-function-). See Performing Steady-State Calcula-

RMS DPM n

(in the Steady Statistics... or Unsteady Statistics... category) is the root mean square value of a discrete

phase variable n (for example, Volume Fraction). See Performing Steady-State Calculations (p. ) and

Rothalpy

(in the Temperature... category) is defined as

(.)

where  is the enthalpy,

is the relative velocity magnitude, and  is the magnitude of the rota-

tional velocity

.

(in the Phase Interaction... category) is the saturation temperature of the n th mass transfer mechanism

that you defined.This item is available only for the evaporation-condensation model. See Including Semi-

Mechanistic Boiling (p. ) for more information about the semi-mechanistic boiling model.

Scalar-n

(in the User Defined Scalars... category) is the value of the

Scalar-n

th scalar quantity you have defined as a user-

defined scalar. See the Fluent Customization Manual for more information about user-defined scalars.

(in the Pdf... category) is one of two parameters that describes the species mass fraction and temperature

for a laminar flamelet in mixture fraction spaces. It is defined as

(.)

where  is the mixture fraction and

is a representative diffusion coefficient (see The Flamelet

Concept in the Theory Guide  for details). Its unit quantity is time-inverse.

Scalar Mass Fraction of species-n

(in the Premixed Combustion... category) is the mass fraction of the species-n in the PDF mixture that

is solved as a transported scalar in the partially-premixed FGM model. (The name of the species will replace

species-n in Scalar Mass Fraction of species-n ).

(in the Radiation... category) is the property of a medium that describes the amount of scattering of

thermal radiation per unit path length for propagation in the medium. It can be interpreted as the inverse

of the mean free path that a photon will travel before undergoing scattering (if the scattering coefficient

does not vary along the path).The unit quantity for Scattering Coefficient is length-inverse.

(in the Pdf... category) is the mean ratio of the secondary stream mass fraction to the sum of the fuel,

secondary stream, and oxidant mass fractions. It is the secondary-stream conserved scalar that is calculated

by the non-premixed combustion model. See Definition of the Mixture Fraction in the Theory Guide .

(in the Pdf... category) is the variance of the secondary stream mixture fraction that is solved for in the

non-premixed combustion model. See Definition of the Mixture Fraction in the Theory Guide .

(in the Temperature... category) is available when any of the species models are active and displays only

the thermal (sensible) enthalpy.

Sensitivity to Body Force X-Component (Cell Values), Sensitivity to Body Force Y-Component (Cell Values),

and Sensitivity to Body Force Z-Component (Cell Values)

(in the Sensitivities... category) are the components of the adjoint velocity primitive field.These fields

can be interpreted as the magnitude of the sensitivity of the observable to components of a body force

per unit volume. Consider a body force distribution, expressed as a force per unit volume.The volume in-

tegral of the vector product of that distribution with the components of this field gives a first-order estimate

of the net effect of the body force on the observation.

(in the Sensitivities... category) is available when the energy adjoint equation is solved and is defined on

walls where a heat flux boundary condition is imposed.The field shows the sensitivity of the observation

of interest to variations in the boundary heat flux through the wall. Its properties are analogous to those

of Sensitivity to Boundary Temperature.

(in the Sensitivities... category) is defined on boundaries where there is a user-specified pressure as part

of a boundary condition, such as on a pressure outlet.The field shows the sensitivity of the observation

of interest to variations in the boundary pressure across the flow boundary. It is interesting to note that

even though the original boundary condition specification may be for a uniform pressure on the domain

boundary, the effect of a non-uniform pressure perturbation is available,The effect of any specific

boundary pressure change can be estimated as an integral of the product of the change to the pressure

with the plotted sensitivity field.Viewing this field will also indicate whether or not the assumption of a

uniform pressure is adequate for the simulation.

boundaries where a temperature boundary condition is applied.This includes walls, velocity inlets, mass-

flow inlets, pressure inlets, and pressure outlets where a backflow temperature may be specified.The field

shows the sensitivity of the observation of interest to variations in the boundary temperature across the

boundaries. Note that even if the original boundary condition specification is for a uniform temperature

on the boundary, the effect of a non-uniform temperature perturbation is available.The effect of any

specific boundary temperature change can be estimated as an integral of the product of the change to

the temperature with the plotted sensitivity field.This field can be used to indicate whether or not the

assumption of a uniform temperature is adequate for the simulation.

Sensitivity to Boundary X-Velocity, Sensitivity to Boundary Y-Velocity, and Sensitivity to Boundary Z-

Velocity

(in the Sensitivities... category) are defined on those boundaries where a user-specification of a boundary

velocity is made for the original flow calculation.This includes no-slip walls.The field shows how sensitive

the observable of interest is to changes in the boundary velocity at any point. It is interesting to note that

even though the original boundary condition specification may be for a uniform velocity on the domain

boundary, the effect of a non-uniform velocity perturbation is available,The effect of any specific boundary

velocity change can be estimated as an integral of the vector product of the change to the velocity with

the plotted sensitivity field. A plot of this quantity on a velocity inlet, for example, can be very useful for

assessing whether or not the inlet is positioned too close to key parts of the system.That is, it addresses

the question of whether or not the flow domain is too small to achieve a successful computation of the

performance measure of interest.Viewing this field will also indicate whether or not the assumption of a

uniform inflow is adequate.

(in the Sensitivities... category) is available when the energy adjoint equation is solved and is the primitive

adjoint temperature field. It can be interpreted as the sensitivity of the observable with respect to thermal

energy sources or sinks per unit volume in the domain.

(in the Sensitivities... category) is provided as a convenient tool for identifying portions of the flow domain

where the introduction of blockages or obstructions in the flow can affect the observation of interest.

Consider a blockage in the flow that generates a reaction force on the flow that is proportional to the

local flow speed, and acting in the opposite direction to the local flow:

where  is a local

coefficient for the reaction force.The local contribution of this force on the observation of interest is de-

termined by the vector product of this force with the adjoint velocity field.The flow blockage field that is

plotted is

, namely the negative of the vector product of the flow velocity and the adjoint velocity

(Cell Value).

Sensitivity to Mass Sources (Cell Values)

(in the Sensitivities... category) is the primitive adjoint pressure field.This field can be interpreted as the

sensitivity of the observable with respect to mass sources or sinks in the domain. Consider a mass source

/ sink distribution, expressed as mass flow rate per unit volume.The volume integral of that distribution,

weighted by the local value of this field, gives the effect of the sources / sinks on the observation.When

plotted on a boundary, this field indicates the effect of the addition or removal of fluid from the domain

upon the quantity of interest. It is important to note that in this scenario the effect of the momentum of

the fluid that is added or removed is not taken into account.The boundary velocity sensitivity should be

plotted if that effect is also of interest.

Sensitivity to Viscosity

(in the Sensitivities... category) shows the sensitivity of the quantity of interest to variations in the turbulent

effective viscosity for a turbulent problem, or the laminar viscosity in a laminar case.The sensitivity is

normalized by the cell volume to account for cell size variations in the mesh.

(in the Sensitivities... category) is the magnitude of the sensitivity of the observable with respect to a

deformation applied to the mesh (both boundary and interior mesh).When plotted on the surface of a

body the locations where this quantity is large indicates where small changes to the surface shape can

have a large effect on the observable of interest. If the shape sensitivity magnitude is small then the effect

of shape changes in this region can be expected to have a small effect on the observable of interest.When

viewing this field, it is often observed that the magnitude varies by many orders of magnitude. Contour

plots will clearly draw attention to regions with the highest sensitivity (often sharp edges and corners).

However, it should be remembered that a relatively small surface movement that is distributed over a

large area can have a cumulative effect that is large.

Shape Sensitivity X-Component, Shape Sensitivity Y-Component, and Shape Sensitivity Z-Component

(in the Sensitivities... category) are the individual components of the sensitivity of the observable of interest

with respect to the mesh node locations. It is plotted as cell data and is computed as the average of the

nodal sensitivities for a given cell, divided by the cell volume. Note that for this discrete adjoint solver the

sensitivity of the result with respect to node locations both on and off boundaries is computed.The nor-

malization by cell volume indicates that the fields that are plotted are the weighting factors for a continuous

spatial deformation field. (Note that the nodal sensitivity data itself is used when mesh morphing is per-

formed, and predictions about the effect of shape changes are made.)

(in the Turbulence... category) is the shielding function

used as part of the Stress-Blended Eddy

Simulation turbulence model and the Shielded Detached Eddy Simulation turbulence model. For details,

see Stress-Blended Eddy Simulation (SBES) and Shielded Detached Eddy Simulation (SDES) in the Fluent

Theory Guide, as well as Including the SDES or SBES Model with BSL, SST, and Transition SST Models (p. ).

Sigma XX, Sigma YY, Sigma XY, Sigma ZZ, Sigma YZ, Sigma XZ,

(in the Structure... category) are the components of the stress tensor.These variables are intended only

for solid zones and/or their adjacent walls in intrinsic fluid-structure interaction (FSI) simulations.

Site fraction of soot species-n

(in the Soot... category) is the ratio of moles of a soot species over the total moles of all soot species. (The

name of the soot species will replace soot species-n in Site fraction of soot species-n.) This

quantity is available only with the Method of Moments model that uses the Detailed CHEMKIN Format

soot mechanism.

(in the Wall Fluxes... category) is a nondimensional parameter defined as the ratio of the wall shear stress

and the reference dynamic pressure

(.)

where

is the wall shear stress, and

and

are the reference density and velocity defined

in the Reference Values Task Page (p. ). For multiphase models, this value corresponds to the

(in the Wall Fluxes... category) is the rate of solar heat transfer through the control surface. Heat flux out

of the domain is negative and heat flux into the domain is positive.

Solidification/Melting...

contains quantities related to solidification and melting.

Soot...

contains quantities related to the Soot model, which is described in Soot Formation (p. ).

(in the Soot... category) is the mass per unit volume of soot.The unit quantity is density. See Fuel NOx

Formation in the Theory Guide  for details.

Soot Mean Diameter

(in the Soot... category) is the average diameter of the soot particles.This quantity is available only with

Soot Surface Area

(in the Soot... category) is the total surface area of the soot particles.This quantity is available only with

(in the Soot... category) is the volume fraction of soot.

(in the Properties... category) is the acoustic speed. It is computed from

. Its unit quantity is velocity.

Important

Note that for the real gas models the sound speed is computed accordingly by the ap-

propriate equation of state formulation.

Important

(in the Acoustics... category) is the time derivative of the Sound Pressure. It is available only when the

acoustics wave equation model is used. Its unit quantity is pressure divided by time.

(in the Acoustics... category) is the acoustic pressure, resulting from the acoustics wave equation. It is

available only when the acoustics wave equation model is used. Its unit quantity is pressure.

(in the Acoustics... category) is the acoustic potential, which is a potential of the acoustics particle velocity,

resulting from the acoustics wave equation. It is available only when the acoustics wave equation model

is used. Its unit quantity is velocity times length.

(in the Acoustics... category) is the marker showing a sponge region of the acoustics wave equation. It is

available only when the acoustics wave equation model is used.

(in the Acoustics... category) is the original model source term of the acoustics wave equation, before the

application of the time filter. It is available only when the acoustics wave equation model is used. Its unit

quantity is square of velocity divided by time.

(in the Acoustics... category) is the marker showing a masking region of the model source term of the

acoustics wave equation. It is available only when the acoustics wave equation model is used.

(in the Acoustics... category) is the model source term of the acoustics wave equation, smoothed by the

time filter. It is available only when the acoustics wave equation model is used. Its unit quantity is square

of velocity divided by time.

(in the Mesh... category) is the normalized (dimensionless) coordinate in the spanwise direction, from hub

to casing. Its value varies from  to .

species-n Source Term

(in the Species... category) is the source term in each of the species transport equations due to reactions.

The unit quantity is always kg/m3-s.

includes quantities related to species transport and reactions.

(in the Turbulence... category) is the rate of dissipation of turbulence kinetic energy in unit volume and

time. Its unit quantity is time-inverse.

(in the Properties... category) is the thermodynamic property of specific heat at constant pressure. It is

defined as the rate of change of enthalpy with temperature while pressure is held constant. Its unit

quantity is specific-heat.

(in the Properties... category) is the ratio of specific heat at constant pressure to the specific heat at constant

volume.

(in the Properties... category) is the temperature of the gas phase at which the derivative of pressure with

respect to molar volume becomes positive.The spinodal temperature defines the point beyond which the

equation of state is no longer valid. If the temperature of your case approaches the spinodal temperature

in some regions, this indicates that the flow conditions in these regions probably fall inside the saturation

dome.The Spinodal Temperature is available only with the Cubic Equation of State Real Gas models.

SPL for Octave Band at x Hz (dB)

(in the Acoustics... category) is the surface pressure level (in decibels) of the standard technical octave

band at the octave central frequency x, as calculated by the Acoustic Sources FFT Dialog Box (p. ). See

FFT of Acoustic Sources: Band Analysis and Export of Surface Pressure Spectra (p. ) for details. Note that

the transformation to the decibel units is done by default using the standard acoustic reference pressure

value of  x - Pa; you can change this value using the Acoustics Model Dialog Box (p. ).

SPL for /-Octave Band at x Hz (dB)

(in the Acoustics... category) is the surface pressure level (in decibels) of the standard technical /-octave

band at the /-octave central frequency x, as calculated by the Acoustic Sources FFT Dialog Box (p. ).

See FFT of Acoustic Sources: Band Analysis and Export of Surface Pressure Spectra (p. ) for details. Note

that the transformation to the decibel units is done by default using the standard acoustic reference

pressure value of  x - Pa; you can change this value using the Acoustics Model Dialog Box (p. ).

SPL for Const Width Band n (dB)

(in the Acoustics... category) is the surface pressure level (in decibels) of the user-defined constant band

n, as calculated by the Acoustic Sources FFT Dialog Box (p. ). See FFT of Acoustic Sources: Band Analysis

and Export of Surface Pressure Spectra (p. ) for details. Note that the transformation to the decibel units

is done by default using the standard acoustic reference pressure value of  x - Pa; you can change this

value using the Acoustics Model Dialog Box (p. ).

(in the Pressure... category) is the static pressure of the fluid. It is a gauge pressure expressed relative to

the prescribed operating pressure.The absolute pressure is the sum of the Static Pressure and the oper-

ating pressure. Its unit quantity is pressure.

(in the Temperature... and Premixed Combustion... categories) is the temperature in the fluid / solid. Its

unit quantity is temperature. For a wall or shadow wall surface, the Static Temperature is the temperature

of the adjacent fluid / solid cells; for a shell surface (see Postprocessing Shells (p. )), it is the temperature

of the shell layer cells on the c0 side (that is, the side closer to the associated wall surface).

Note that Static Temperature will appear in the Premixed Combustion... category only for adia-

batic premixed combustion calculations. See Postprocessing for Premixed Combustion Calcula-

Steady Statistics...

includes mean and root mean square error (RMSE) values of solution variables and custom field functions

derived from steady state flow calculations (with Data Sampling for Steady Statistics enabled).

(in the Derivatives... category) relates shear stress to the viscosity. Also called the shear rate (  in Equa-

tion . (p. )), the strain rate is related to the second invariant of the rate-of-deformation tensor . Its

unit quantity is time-inverse. In 3D Cartesian coordinates, the strain rate,

, is defined as

(.)

Stream Function

(in the Velocity... category) is formulated as a relation between the streamlines and the statement of

conservation of mass. A streamline is a line that is tangent to the velocity vector of the flowing fluid. For

a 2D planar flow, the stream function,

, is defined such that

(.)

constant values of stream function defining two streamlines is the mass rate of flow between the

streamlines.

The accuracy of the stream function calculation is determined by the text command /dis-

play/set/n-stream-func.

(in the Premixed Combustion... category) is a nondimensional parameter that is defined as the probability

of unquenched flamelets (  in Equation . in the Theory Guide ).

(in the Properties... category) has a value of  if the flow condition is subcritical and  if the flow condition

is supercritical and is available with the Cubic Equation of State Real Gas models.

(in the Turbulence... category) is the turbulence dissipation rate of the unresolved eddies,

, only

active for the LES and Kinetic Energy Subgrid-Scale Model. It is defined as

(.)

Its unit quantity is turbulent-energy-diss-rate.

(in the Turbulence... category) is used in the calculation of the subgrid-scale turbulent flux of a scalar ,

see Subgrid-Scale Models in the Theory Guide, Equation ..

(in the Turbulence... category) is used in the calculation of the subgrid-scale turbulent flux for Species

(see Subgrid Dynamic Prandtl Number).

(in the Turbulence... category) is the Smagorinsky model constant as determined by the dynamic procedure

described in Dynamic Smagorinsky-Lilly Model in the Theory Guide ). Additional information with respect

to the Embedded LES (E-LES) model can be found in Postprocessing for Turbulent Flows (p. ).

(in the Turbulence... category) is a mixing length for subgrid scales of the LES turbulence model (defined

as

in Equation . in the Theory Guide ).

(in the Turbulence... category) is the turbulence kinetic energy per unit mass of the unresolved eddies,

, calculated using a transport equation, only active for the LES and Kinetic Energy Subgrid-Scale Model.

It is defined as

(.)

Additional information with respect to the Embedded LES (E-LES) model can be found in Postpro-

cessing for Turbulent Flows (p. ). Its unit quantity is turbulent-kinetic-energy.

Subgrid Test–Filter Length

(in the Turbulence... category) is the test filter width

described in Dynamic Smagorinsky-Lilly Model in

the Theory Guide ). Additional information with respect to the Embedded LES (E-LES) model can be found

in Postprocessing for Turbulent Flows (p. ).

(in the Turbulence... category) is the turbulent (dynamic) viscosity of the fluid calculated using the LES

turbulence model. It expresses the proportionality between the anisotropic part of the subgrid-scale stress

tensor and the rate-of-strain tensor. (See Equation . in the Theory Guide .) Its unit quantity is viscosity.

(in the Turbulence... category) is the ratio of the subgrid turbulent viscosity of the fluid to the laminar

viscosity, calculated using the LES turbulence model.

(in the Turbulence... category) is the turbulence kinetic energy of filtered eddies,

, only active for the

LES and Kinetic Energy Subgrid-Scale Model. It is defined as

(.)

with

being the normal components of the Leonard stress.

Its unit quantity is turbulent-kinetic-energy

(in the Acoustics... category) is the Acoustic Power per unit area generated by boundary layer turbulence

acoustics model is being used. Its unit quantity is power per area.

(in the Acoustics... category) is the Acoustic Power per unit area generated by boundary layer turbulence,

and represented in dB (see Equation . in the Theory Guide ). It is available only when the Broadband

(in the Radiation... category) is used to view the distribution of surface clusters in the domain. Each cluster

has a unique integer number (ID) associated with it.

(in the Species... category) is the rate of

th solid species consumption/deposition. A positive value indicates

corrosion of the solid species on the interface, and a negative value indicates deposition of the solid species.

Surface Coverage of species-n

(in the Species... category) is the amount of a surface species that is deposited on the substrate at a spe-

cific point in time.

Surface Deposition Rate of species-n

(in the Species... category) is the amount of a surface species that is deposited on the substrate. Its unit

Surface dpdt RMS, definition

(in the Acoustics... category) is the RMS value of the time-derivative of static pressure (

). It is

available when the Ffowcs-Williams & Hawkings acoustics model is being used.

(in the Wall Fluxes... category), as defined in ANSYS Fluent, is given by the equation

(.)

is the reference temperature defined in the Reference Values Task Page (p. ). Note that

is a constant value that should be representative of the problem. Its unit quantity is the heat-

transfer- coefficient.

(in the Wall Fluxes... category) is the net incoming radiation heat flux on a surface. Its unit quantity is

(in the Wall Fluxes... category) is a local nondimensional coefficient of heat transfer defined by the

equation

(.)

(in the Wall Fluxes... category) is a nondimensional coefficient of heat transfer defined by the equation

(.)

are reference values of density and velocity defined in the Reference Values Task Page (p. ),

and

is the specific heat at constant pressure.

Swirl Pull Velocity

(in the Solidification/Melting... category) is the tangential-direction component of the pull velocity for

the solid material in a continuous casting process. Its unit quantity is velocity.

Swirl Velocity

(in the Velocity... category) is the tangential-direction component of the velocity in an axisymmetric

swirling flow. See Velocity Reporting Options (p. ) for details.The unit quantity for Swirl Velocity is

velocity. For multiphase models, this value corresponds to the selected phase in the Phase drop-down

list.

Swirl-Wall Shear Stress

(in the Wall Fluxes... category) is the swirl component of the force acting tangential to the surface due to

(in the Velocity... category) is the velocity component in the tangential direction. (See Velocity Reporting

Options (p. ) for details.) The unit quantity for Tangential Velocity is velocity.

indicates the quantities associated with the thermodynamic temperature of a material.

(in the Properties... category) is a parameter ( ) that defines the conduction rate through a material via

Fourier’s law (

). A large thermal conductivity is associated with a good heat conductor and a

small thermal conductivity with a poor heat conductor (good insulator). Its unit quantity is thermal-con-

ductivity. Note that when postprocessing solid material properties, the Thermal Conductivity will be dis-

played as zero if an anisotropic thermal conductivity model is being used for a solid material.

(in the Species... category) is the thermal diffusion coefficient for the

th species (

in Equa-

tion . (p. ), Equation . (p. ), and Equation . (p. )). Its unit quantity is viscosity.

Time Step

(in the Residuals... category) is the local time step of the cell,

, at the current iteration level. Its unit

quantity is time.

(in the Species... category) is the factor by which the time step is reduced for the stiff chemistry solver

(available in the density-based solver only).The time step is scaled down based on an eigenvalue and

positivity analysis.

(in the Potential... category) is the summation of the Joule and Faradaic heat sources.The total heat source

due to electrochemical chemical reactions is added to the energy equation.

(in the Temperature... category) is the total energy per unit mass. Its unit quantity is specific-energy. For

all species models, plots of Total Energy include the sensible, chemical and kinetic energies. For multiphase

models, this value corresponds to the selected phase in the Phase drop-down list.

where

is the Enthalpy, as defined in Equation .

in the Theory Guide , and  is the velocity magnitude. Its unit quantity is specific-energy. For all species

models, plots of Total Enthalpy consist of the sensible, chemical and kinetic energies. For multiphase

(in the Temperature... category) is the difference between Total Enthalpy and the reference enthalpy,

, where

is the reference enthalpy defined in the Reference Values Task Page (p. ).

However, for non-premixed and partially premixed models, Total Enthalpy Deviation is the difference

between Total Enthalpy and total adiabatic enthalpy (total enthalpy where no heat loss or gain occurs).

The unit quantity for Total Enthalpy Deviation is specific-energy. For multiphase models, this value

corresponds to the selected phase in the Phase drop-down list.

(in the Pressure... category) is the pressure at the thermodynamic state that would exist if the fluid were

brought to zero velocity and zero potential. For compressible flows, the total pressure is computed using

isentropic relationships. For constant

, this reduces to:

(.)

For incompressible flows (constant density fluid), we use Bernoulli’s equation,

, where

is the local dynamic pressure. Its unit quantity is pressure.

Important

(.)

, where

Important

Note that in the postprocessing, the total pressure is presented as gauge pressure,

for compressible and incompressible flows. If the total absolute pressure is needed,

then add the value of the reference pressure to the total gauge pressure.

(in the Potential... category) is the total rate of solid species consumption/deposition. A positive value

indicates corrosion of the solid species on the interface, and a negative value indicates deposition of the

solid species. It’s computed as the sum of the surface corrosion rates (Surface Corrosion Rates of spe-

cies-n  reported under the Species category) of all species.

(in the Wall Fluxes... category) is the rate of total heat transfer through the control surface. It is calculated

by the solver according to the boundary conditions being applied at that surface. By definition, heat flux

out of the domain is negative, and heat flux into the domain is positive.The unit quantity for Total Surface

Heat Flux is heat-flux.

(in the Temperature... category) is the temperature at the thermodynamic state that would exist if the

fluid were brought to zero velocity. For compressible flows, the total temperature is computed from the

total enthalpy using the current

method (specified in the Create/Edit Materials Dialog Box (p. )). For

incompressible flows, the total temperature is equal to the static temperature, unless kinetic energy is

explicitly added.The unit quantity for Total Temperature is temperature.

Transmitted Radiation Flux (Band-n)

(in the Wall Fluxes... category) is the amount of radiative heat flux transmitted by a semi-transparent wall

Transmitted Visible Solar Flux,Transmitted IR Solar Flux

(in the Wall Fluxes... category) is the amount of solar heat flux transmitted by a semi-transparent wall or

porous jump boundary for a visible or infrared radiation.

includes quantities related to turbulence. See Modeling Turbulence (p. ) for information about the tur-

bulence models available in ANSYS Fluent.

(in the Turbulence... category) is the ratio of the magnitude of the RMS turbulent fluctuations to the ref-

erence velocity:

(.)

where  is the turbulence kinetic energy and

is the reference velocity specified in the Reference

Values Task Page (p. ). The reference value specified should be the mean velocity magnitude for

the flow. Note that turbulence intensity can be defined in different ways, so you may want to use

a custom field function for its definition. See Custom Field Functions (p. ) for more information.

(in the Turbulence... category) is the turbulent dissipation rate. Its unit quantity is turbulent-energy-diss-

rate.This quantity is available for the k-epsilon and k-omega based turbulence models, where the epsi-

lon/omega relationship is defined as

(.)

(.)

(in the Premixed Combustion... category) is the turbulent flame speed computed by ANSYS Fluent using

Equation . in the Theory Guide . Its unit quantity is velocity.

(in the Turbulence... category) is the turbulence kinetic energy per unit mass defined as

(.)

(in the Reactions... category) is the rate of progress of the

th reaction computed by Equation . or

Equation . (in the Theory Guide ). For the “eddy-dissipation” model, the value is the same as the Rate

of Reaction-n. For the “finite-rate” model, the value is zero.

(in the Turbulence... category) is a nondimensional quantity defined as

(.)

where  is turbulence kinetic energy,

is the distance to the nearest wall, and

is the laminar

(in the Turbulence... category) is the turbulent viscosity of the fluid computed using the turbulence

model. Its unit quantity is viscosity. For multiphase models, this value corresponds to the selected phase

in the Phase drop-down list. Additional information with respect to the Embedded LES (E-LES) model can

be found in Postprocessing for Turbulent Flows (p. ).

(in the Turbulence... category) is used in the -

transition model.See Transport Equations for the k-

kl-ω Model in the Theory Guide for more details (Equation . ).

transition model. See Transport Equations for the k-

(in the Turbulence... category) is the ratio of turbulent viscosity to the laminar viscosity. Additional inform-

ation with respect to the Embedded LES (E-LES) model can be found in Postprocessing for Turbulent

User Memory <n>

(in the User Defined Memory... category) is the value of the quantity in the

th user-defined memory

location.

User Node Memory <n>

th user-defined node memory

location.

(in the Premixed Combustion... category) is the mass fraction of unburnt fuel.This function is available

Unsteady Statistics...

derived from transient flow calculations.

includes quantities that have been allocated to a user-defined memory location. See the separate Fluent

Customization Manual for details about user-defined memory.

User-Defined Scalars...

includes quantities related to user-defined scalars. See the separate Fluent Customization Manual for in-

formation about using user-defined scalars.

(in the Turbulence... category) is the

stress.

stress.

Resolved UV Reynolds Stress

(in the Turbulence... category) is defined as:

(.)

at time

stress.

stress.

(.)

at time

. This variable is only available if you enable Data Sampling for Time Statistics in the

Run Calculation Task Page (p. ). Time

represents the time Data Sampling for Time Statistics

is first enabled, which is not necessarily the first timestep.

stress.

Resolved UW Reynolds Stress

(.)

at time

Variance of Species

(in the NOx... category) is the variance of the mass fraction of a selected species in the flow field. It is cal-

culated from Equation . in the Theory Guide .

Variance of Species ,Variance of Species

(in the NOx... category) are the variances of the mass fractions of the selected species in the flow field.

They are each calculated from Equation . in the Theory Guide .

Variance of Temperature

(in the NOx... category) is the variance of the normalized temperature in the flow field. It is calculated from

includes the quantities associated with the rate of change in position with time.The instantaneous velocity

of a particle is defined as the first derivative of the position vector with respect to time,

, termed

the velocity vector,

.

(in the Velocity... category) is defined as follows:

For a 2D model,

(.)

For a 2D or axisymmetric model,

, termed

.

(.)

(.)

For a 3D model,

(.)

(in the Velocity... category) is the speed of the fluid. Its unit quantity is velocity. For multiphase models,

this value corresponds to the selected phase in the Phase drop-down list.

(in the Phases... category) is the volume fraction of the selected phase in the Phase drop-down list.

(in the Radiation... category) is the spherical mean absorbed radiation and, for a single spectral band, can

be defined as:

(.)

where  is the radiation intensity and  is the absorption coefficient.

(in the Radiation... category) is the spherical mean emitted radiation and, for a single spectral band, can

be defined as.

(.)

where  is the blackbody fraction,

is the Stefan-Boltzmann constant,

is the absorption coefficient.

(in the Velocity... category) is the magnitude of the vorticity vector.Vorticity is a measure of the rotation

of a fluid element as it moves in the flow field, and is defined as the curl of the velocity vector:

(.)

stress.

stress.

Resolved VW Reynolds Stress

(.)

at time

(.)

at time

(in the Wall Fluxes… category) is defined as:

(.)

where  is the surface heat flux,

is the wall face temperature, and

is the wall adjacent cell

(in the Temperature… category) is the temperature of the fluid cell adjacent to the wall.

(in the Wall Film… category) is the fraction of the wall surface covered by the wall film.

(in the Wall Film… category) is the face pressure of the wall film.

(in the Wall Film… category) is the height of the wall film.

(in the Wall Film… category) is the heat flux of the wall film to the wall.

(in the Wall Film… category) is the mass flux impinging on the wall film.

(in the Wall Film… category) is the mass of the wall film (in units of mass).

(in the Wall Film… category) is the temperature of the wall film.

(in the Wall Film… category) is the velocity magnitude of the wall film.

Wall Film X-Velocity

(in the Wall Film… category) is the x-component of the velocity of the wall film.

Wall Film Y-Velocity

(in the Wall Film… category) is the y-component of the velocity of the wall film.

Wall Film Z-Velocity

(in the Wall Film… category) is the z-component of the velocity of the wall film.

includes quantities related to forces and heat transfer at wall surfaces.

is generally defined by the equation

(.)

where

is the near-wall turbulence velocity scale,

is the viscous heating

(included only for variable density flows, Equation . in the Fluent Theory Guide),

is the dimen-

sionless law-of-the-wall temperature defined for the standard wall functions in Equation . in

the Fluent Theory Guide. For the enhanced wall treatment, the combined forms for

and

(Equation . and Equation . in the Fluent Theory Guide) are replaced by the corresponding

functions obtained using the blending of Kader, explained in Enhanced Wall Treatment for Momentum

and Energy Equations in the Fluent Theory Guide.

Wall Irradiation Flux.Normalized Std Deviation

(in the Radiation... category) is the statistical standard deviation for the hemispherical mean irradiation

flux.

Wall Leidenfrost Temperature

(in the Wall Film… category) is the wall temperature at which the insulating vapor layer fully covers the

hot wall preventing the liquid from boiling rapidly.

Film Mass Fraction of material-i

(in the Wall Film... category) is the mass fraction of the discrete phase material i in the wall film. (The name

of the material will replace material-i  in Film Mass Fraction of material-i .)

Wall Shear Stress

(in the Wall Fluxes... category) is the force acting tangential to the surface due to friction. Its unit quantity

is pressure. For multiphase models, this value corresponds Equation . in the Fluent Theory Guide to

the selected phase in the Phase drop-down list.

(in the Temperature... category) is the temperature on a surface (including wall surfaces, shadow wall

surfaces, and shell surfaces). For an illustration of such surfaces for thin walls and shells, see Figure . : A

Thin Wall (p. ) and Figure . : A Boundary Wall with Shell Conduction (p. ), respectively.

(in the Temperature... category) is for thin walls only, and reports the temperature on the surface that is

separated from the fluid / solid cells by the wall thickness, as shown in Figure . : A Thin Wall (p. ).

Note that the wall thermal boundary conditions are applied on this surface.

Wall Yplus

(in the Turbulence... category) is a nondimensional parameter defined by the equation

(.)

where

is the friction velocity,

is the distance from point  to the wall,

is the fluid

density, and  is the fluid viscosity at point . See Near-Wall Treatments for Wall-Bounded Turbulent

Flows in the Theory Guide  for details. For multiphase models, this value corresponds to the selected

phase in the Phase drop-down list.

Wall Ystar

(.)

where

is the turbulence kinetic energy at point ,

is the fluid density, and  is the fluid viscosity at point . See Near-Wall Treatments for Wall-

Bounded Turbulent Flows in the Theory Guide  for details.

stress.

X-Coordinate,Y-Coordinate, Z-Coordinate

stress.

(in the Mesh... category) are the Cartesian coordinates in the -axis,

axis, and -axis directions respectively.

The unit quantity for these variables is length.

X Displacement,Y Displacement, Z Displacement

(in the Structure... category) are the components of the displacement.These variables are intended only

X Face Area,Y Face Area, Z Face Area

(in the Mesh... category) are the components of the face area vector for noninternal faces (that is, faces

that only have c0 and no c1).The values are stored on the face itself and used when required.These

variables are intended only for zone surfaces and not for other surfaces created for postprocessing.

X Pull Velocity,Y Pull Velocity, Z Pull Velocity

(in the Solidification/Melting... category) are the ,

, and  components of the pull velocity for the solid

material in a continuous casting process.The unit quantity for each is velocity.

X Velocity,Y Velocity, Z Velocity

(in the Velocity... category) are the components of the velocity vector in the -axis,

axis, and -axis

directions, respectively.The unit quantity for these variables is velocity. For multiphase models, these

values correspond to the selected phase in the Phase drop-down list.

X-Vorticity,Y-Vorticity, Z-Vorticity

(in the Velocity... category) are the ,

, and  components of the vorticity vector.

X-Wall Shear Stress,Y-Wall Shear Stress, Z-Wall Shear Stress

(in the Wall Fluxes... category) are the ,

, and  components of the force acting tangential to the surface

due to friction.The unit quantity for these variables is pressure. For multiphase models, these values cor-

respond to the selected phase in the Phase drop-down list.

In addition to the basic field variables provided by ANSYS Fluent (and described in Alphabetical Listing

of Field Variables and Their Definitions (p. )), you can also define your own field functions to be used

in conjunction with any of the commands that use these variables (contour and vector display, XY plots,

and so on). This capability is available with the Custom Field Function Calculator Dialog Box (p. ).

You can use the default field variables, previously defined calculator functions, and calculator operators

to create new functions. (Several sample functions are described in Sample Custom Field Func-

tions (p. ).)

Any field functions that you define will be saved in the case file the next time that you save it. You can

also save your custom field functions to a separate file (as described in Manipulating, Saving, and

Loading Custom Field Functions (p. )), so that they can be used with a different case file.

Important

Note that all custom field functions are evaluated and stored in SI units.

Any solver-defined flow variables that you use in your field-function definition will be auto-

matically converted if they are not already in SI units, but you must be careful to enter con-

stants in the appropriate units. Note also that explicit node values are not available for custom

field functions; all node values for these functions will be computed by averaging the values

in the surrounding cells, as described in Node Values (p. ).

... Creating a Custom Field Function

... Manipulating, Saving, and Loading Custom Field Functions

... Sample Custom Field Functions

To create your own field function, you will use the Custom Field Function Calculator Dialog Box (p. )

(Figure . : The Custom Field Function Calculator Dialog Box (p. )). This dialog box allows you to

define field functions based on existing functions, using simple calculator operators. Any functions

that you define will be added to the list of default flow variables and other field functions provided

New...

Important

Recall that you must enter all constants in the function definition in SI units.

Custom Field Functions

Figure . : The Custom Field Function Calculator Dialog Box

The steps for creating a custom field function are as follows:

. Use the calculator buttons and the Field Functions list and Select button to specify the function definition,

as described below. (As you select each item from the Field Functions list or click a button in the calcu-

lator keypad, its symbol will appear in the Definition text entry box.You cannot edit the contents of this

box directly; if you want to delete part of a function, use the DEL button on the keypad.)

Important

Important

The range of integers and real numbers that can be stored is as follows:

Note that using a number less than 1e- may produce inaccurate results, while values

less than 1e- will produce a result of zero.

. Specify the name of the function in the New Function Name field.

Important

Be sure that you do not specify a name that is already used for a standard field function

(for example, velocity-magnitude); you can see a complete list of the predefined

field functions in ANSYS Fluent by selecting the display/contours text command

and viewing the available choices for contours of.

. Click the Define button.

When you click Define, the solver will create the function and add it to the list of Custom Field

Functions within the drop-down list of available field functions. The Define push button is grayed out

after you create a new function or if the Definition text entry box is empty.

Should you decide to rename or delete the function after you have completed the definition, you can

do so in the Field Function Definitions Dialog Box (p. ), which you can open by clicking on the

Manage... push button. See Manipulating, Saving, and Loading Custom Field Functions (p. ) for

details.

.... Using the Calculator Buttons

Your function definition can include many basic calculator operations (for example, addition, subtrac-

tion, multiplication, square root). When you select a calculator button (by clicking on it), the appropriate

symbol will appear in the Definition text entry box. The meaning of the buttons is straightforward;

they are similar to the buttons you would find on any standard calculator. You should, however, note

The CE/C button will clear the entire Definition and the New Function Name, if you have entered one.

The DEL button will delete only the last entry in the Definition text entry box.You can use DEL to delete

characters one at a time, starting with the last one entered.

To obtain the inverse trigonometric functions arcsin, arccos, and arctan, click the INV button before se-

lecting sin, cos, or tan.

The ABS button yields the absolute value of the number that follows it. Likewise, the ln button yields the

natural logarithm of the number that follows it, and the log10 button yields the base  logarithm function

of the number that follows it.

Important

log10 and ln will be calculated for values greater than . For values less than or equal

to , the resultant value will be zero.

The PI button represents  and the e button represents the base of the natural logarithm system (which

is approximately equal to

).

.... Using the Field Functions List

Your function definition can include any of the field functions defined by the solver (and listed in

Alphabetical Listing of Field Variables and Their Definitions (p. )) or by you. You can also use any

report definitions that you have created (see Monitoring and Reporting Solution Data (p. ) for ad-

ditional information). To include one of these variables/functions in your function definition, select

it in the Field Functions drop-down list and then click the Select button below the list. The symbol

for the selected item will appear in the Definition text entry box (for example, p will appear if you

select Static Pressure).

Note

Note

If a custom field function definition uses a report definition, then it cannot be exported

to a file.

Once you have defined your field functions, you can manipulate them using the Field Function

Definitions Dialog Box (p. ) (Figure . : The Field Function Definitions Dialog Box (p. )). You can

display a function definition to be sure that it is correct, delete the function if you decide that it is in-

correct and must be redefined, or give the function a new name. You can also save custom field

functions to a file or read them from a file. The custom field function file allows you to transfer your

custom functions between case files.

To open the Field Function Definitions Dialog Box (p. ), right-click Custom Field Functions (under

the Parameters & Customization branch of the tree) and select Manage.... You can also click the

Manage... button in the Custom Field Function Calculator Dialog Box (p. ).

Figure . : The Field Function Definitions Dialog Box

The following actions can be performed in the Field Function Definitions Dialog Box (p. ):

To check the definition of a function, select it in the Field Functions list. Its definition will be displayed in

the Definition field.This display is for informational purposes only; you cannot edit it. If you want to change

a function definition, you must delete the function and define it again in the Custom Field Function Calcu-

lator Dialog Box (p. ).

To delete a function, select it in the Field Functions list and click the Delete button.

To rename a function, select it in the Field Functions list, enter a new name in the Name field, and click

the Rename button.

Important

To save all of the functions in the Field Functions list to a file, click the Save... button and specify the file

name in The Select File Dialog Box (p. ).

To read custom field functions from a file that you saved as described above, click the Load... button and

specify the file name in the resulting Select File dialog box. (Custom field function files are valid Scheme

functions, and can also be loaded with the File/Read/Scheme... ribbon tab item, as described in Reading

Scheme Source Files (p. ).)

When you are checking the results of your simulation, you may find it useful to define some of the

following field functions:

To define a function that determines the ratio of static pressure to inlet total pressure, use the relationship

(.)

where  is the static pressure calculated by the solver,

is the inlet total pressure, and

is the

operating pressure for the problem. Use the solver-defined function Static Pressure for , and the

is the

numerical value that you specified for Gauge Total Pressure in the Pressure Inlet Dialog Box (p. )

for

. Specify the value of the operating pressure to be the value that you set in the Operating

Conditions Dialog Box (p. ). As discussed in Operating Pressure (p. ), all pressures in ANSYS

Fluent are gauge pressures relative to the operating pressure. If the operating pressure is zero, as is

generally the case for compressible flow calculations, the expression for the pressure ratio reduces

to

(.)

To define a function that determines the critical velocity ratio

, a parameter that is sometimes used

in turbomachinery calculations, use the relationship

(.)

In this relationship,

is the critical velocity (that is, the velocity that would occur for the same

stagnation conditions if

),

is the ratio of specific heats, and

is the pressure ratio defined

in Equation . (p. ) for which you created your own function. For , ratio of specific heats, select

Specific Heat Ratio (gamma) in the Properties... category. To include

, select Custom Field

Functions... in the first drop-down list under Field Functions, and then select from the second list

the function name that you assigned

.

Suppose you have swirling flow in a pipe, aligned with the  axis, and you want to calculate the flow rate

of angular momentum through a cross-sectional plane:

(.)

You can create a function for the product

, where  is the Radial Coordinate and

is the

Tangential Velocity. Then use the Surface Integrals Dialog Box (p. ) to compute the flow rate of

this quantity.

is the

Important

The custom field function containing model dependent functions (like temperature when

the energy equation is enabled) will be computed only when those models are still active.

Chapter : Parallel Processing

The following sections describe the parallel-processing features of ANSYS Fluent.

.. Introduction to Parallel Processing

.. Starting Parallel ANSYS Fluent Using Fluent Launcher

.. Starting Parallel ANSYS Fluent on a Windows System

.. Starting Parallel ANSYS Fluent on a Linux System

.. Mesh Partitioning and Load Balancing

.. Using General Purpose Graphics Processing Units (GPGPUs) With the Algebraic Multigrid (AMG) Solver

.. Controlling the Threads

.. Checking Network Connectivity

.. Checking and Improving Parallel Performance

Processing in ANSYS Fluent involves an interaction between ANSYS Fluent, a host process, and one or

more compute-node processes. ANSYS Fluent interacts with the host process and the compute node(s)

using a utility called cortex that manages ANSYS Fluent’s user interface and basic graphical functions.

For serial processing, the ANSYS Fluent solver uses only a single compute node. For parallel processing,

a solution is computed using multiple compute nodes that may be executing on the same computer,

or on different computers in a network (Figure . : ANSYS Fluent Architecture (p. )).

Parallel ANSYS Fluent splits up the mesh and data into multiple partitions, then assigns each mesh

partition to a different compute node. The number of partitions is equal to or less than the number of

processors (or cores) available on your compute cluster. The compute-node processes can be executed

on a massively parallel computer, a multiple-CPU workstation, or a network cluster of computers.

Generally, as the number of compute nodes increases, turnaround time for solutions will decrease. This

is referred to as solver “scalability.” However, beyond a certain point, the ratio of network communication

to computation increases, leading to reduced parallel efficiency, so optimal system sizing is important

for simulations.

Parallel Processing

ANSYS Fluent uses a host process that does not store any mesh or solution data. Instead, the host

process only interprets commands from ANSYS Fluent’s graphics-related interface, cortex.

The host distributes those commands to the other compute nodes via a socket interconnect to a single

designated compute node called compute-node-. This specialized compute node distributes the

host commands to any additional compute nodes. Each compute node simultaneously executes the

same program on its own data set. Communication from the compute nodes to the host is possible

only through compute-node- and only when all compute nodes have synchronized with each

other.

Each compute node is virtually connected to every other compute node, and relies on inter-process

communication to perform such functions as sending and receiving arrays, synchronizing, and performing

global operations (such as summations over all cells). Inter-process communication is managed by a

message-passing library. For example, the message-passing library could be a vendor implementation

of the Message Passing Interface (MPI) standard, as depicted in Figure . : ANSYS Fluent Architec-

ture (p. ).

All of the parallel ANSYS Fluent processes (as well as the serial process) are identified by a unique integer

ID. The host collects messages from compute-node- and performs operations (such as printing,

displaying messages, and writing to a file) on all of the data.

... Recommended Usage of Parallel ANSYS Fluent

The recommended procedure for using parallel ANSYS Fluent is as follows:

. Start up the parallel solver. For details, see Starting Parallel ANSYS Fluent on a Windows System (p. )

and Starting Parallel ANSYS Fluent on a Linux System (p. ).

. Read your case file and have ANSYS Fluent partition the mesh automatically upon loading it.

. Review the partitions and perform partitioning again, if necessary. See Checking the Partitions (p. ) for

details on checking your partitions. Note that there are other approaches for partitioning, including

manual partitioning in either the serial or the parallel solver. For details, see Mesh Partitioning and Load

Balancing (p. ).

. Calculate a solution. See Checking and Improving Parallel Performance (p. ) for information on checking

and improving the parallel performance.

Note

Due to limitations imposed by several MPI implementations, ANSYS Fluent performance on

Note

heterogeneous clusters involving either operating system or processor family differences

may not be optimal, and in certain cases cause failures. You are urged to use caution in

such parallel operating environments.

Whether you start ANSYS Fluent either from the Linux or Windows command line with no arguments,

from the Windows Programs menu, or from the Windows desktop, Fluent Launcher will appear (for

Starting Parallel ANSYS Fluent Using Fluent Launcher

details, see Starting ANSYS Fluent Using Fluent Launcher (p. ) in the Getting Started Guide), where

you can specify the dimensionality of the problem (2D or 3D), as well as other options (for example,

whether you want a single-precision or double-precision calculation).

Parallel calculation options can be set up by selecting Parallel under Processing Options in Fluent

Launcher. Once you select the Parallel option, you can also specify the number of processes using the

Processes field under Solver.

If your machines are equipped with appropriate General Purpose Graphical Processing Units (GPGPUs)

you can indicate that these should be used for AMG solver acceleration by setting the GPGPUs per

Machine option. Note that the number of solver processes per machine must be the same for all ma-

chines and that the number of processes per machine must be evenly divisible into the value you specify

for GPGPUs per Machine. That is, for nprocs solver processes running on M machines using ngpgpus

GPGPUS per machine:

Table . : Examples for GPGPUs per Machine (p. ) presents several examples illustrating the relation-

ship between number of machines, number of solver processes, and GPGPUs per machine.

Table . : Examples for GPGPUs per Machine

Example

Example

Example

Number of Machines (M)

Number of Solver Processes (nprocs)

ngpgpus will be ignored and

GPGPU acceleration will be

,

, ,

Valid values for GPGPUs per Machine

(ngpgpus)

disabled (M does not evenly

divide nprocs)

See Using General Purpose Graphics Processing Units (GPGPUs) With the Algebraic Multigrid (AMG)

Solver (p. ) for more information about using GPGPU acceleration.

Activating the Parallel option enables the Parallel Settings tab (visible when you select the Show

More Options button). The Parallel Settings tab allows you to specify settings for running ANSYS

Fluent in parallel.

Specify the interconnect in the Interconnects drop-down list.The default setting is recommended. For a

symmetric multi-processor (SMP) system, the default setting uses shared memory for communication. On

Windows, the best available interconnect is automatically used.

(Linux only) If you prefer to select a specific interconnect, you can choose either ethernet or infini-

band. For more information about these interconnects, see Table . : Supported Interconnects for

Linux Platforms (Per Platform) (p. ), Table . : Available MPIs for Linux Platforms (p. ), and

Table . : Supported MPIs for Linux Architectures (Per Interconnect) (p. ).

Specify the type of message passing interface (MPI) you require for the parallel computations in the MPI

Types field.The list of MPI types varies depending on the selected release and the selected architecture.

There are several options, based on the operating system of the parallel cluster. For more information about

the available MPI types, see Table . : Supported Interconnects for the Windows Platform (p. ) -

Table . : Available MPIs for Windows Platforms (p. ).

Important

It is your responsibility to make sure the interconnects and the MPI types are compatible.

If incompatible inputs are used, Fluent Launcher resorts to using the default values.

(Linux Only) Specify either RSH (remote shell client) or SSH (secure shell client) under Remote Spawn

Command. For more information about setting up your remote shell clients and secure shell clients, see

Setting Up Your Remote Shell and Secure Shell Clients (p. ).

Specify the type of parallel calculation under Run Types:

– Select Shared Memory on Local Machine if the parallel calculations are performed by sharing memory

allocations on your local machine.

– Select Distributed Memory on a Cluster if the parallel calculations will be distributed among

several machines.

You can select Machine Names and enter the machine names directly into the text field as a list.

Machine names can be separated either by a comma or a space. This is not recommended for a

long list of machine names.

Alternatively, you can select File Containing Machine Names to specify a hosts file (a file that

contains the machine names), or you can use the

button to browse for a hosts file.

To edit an existing hosts file, click the

button.

button.

By default, Fluent allocates ranks to machines in contiguous blocks, where the block sizes are as

equal as possible. You can control the per machine block allocation size using the machine X :

Y convention in the hosts specification, where Y is the process block count for machine X. The

process assignment will cycle through the machine list until all processes are allocated in specified

blocks. A fully round-robin assignment of processes can be achieved by setting the machine block

allocation sizes to  (for example, machine1:, machine2:, and so on).

Enable the Select IP Interface option and make a selection from the drop-down list that appears if

you would like to specify the IP interface to be used by the host process. This is equivalent to the

host_ip=host:ip command line option. An example of when you might use this option is when

you are using distributed memory on multiple machines and your security software is dropping the

active socket connections used by ANSYS Fluent (resulting in the following message in the console:

The fl process could not be started. ); while it is preferable to avoid this by creating

an exception for ANSYS Fluent in your security software, you could instead select a suitable IP interface.

For certain platforms, select Use Job Scheduler under Options if the parallel calculations are to be performed

using a designated Job Scheduler (for details, see Setting Parallel Scheduler Options in Fluent Launch-

er (p. )).This also enables the Scheduler tab of Fluent Launcher.

... Setting Parallel Scheduler Options in Fluent Launcher

... Setting Additional Options When Running on Remote Linux Machines

Activating the Use Job Scheduler option under Options in Fluent Launcher enables the Scheduler

tab (visible when you select Show More Options). The Scheduler tab allows you to specify settings

for running ANSYS Fluent with various job schedulers (for example, the Microsoft Job Scheduler for

Windows, or LSF, SGE, and PBS Professional on Linux).

For Windows -bit, with MSMPI or when the Use Remote Linux Nodes option is selected, you can

specify that you want to use the Job Scheduler by selecting the Use Job Scheduler check box under

Options in Fluent Launcher. Once selected, you can then enter a machine name in the Compute

Cluster Head Node Name text field in the Scheduler tab. If you are running ANSYS Fluent on the

head node, then you can keep the field empty. This option translates into the proper parallel command

line syntax for using the Microsoft Job Scheduler (for details, see Starting Parallel ANSYS Fluent with

the Microsoft Job Scheduler (p. )).

If you want ANSYS Fluent to start after the necessary resources have been allocated by the Scheduler,

then select the Start When Resources are Available check box.

For Linux, select the Use Job Scheduler check box under Options to use one of three available job

schedulers in the Scheduler tab.

Select Use LSF to use the LSF load management system with or without checkpointing. If you select Use

Checkpointing, then you can specify a checkpointing directory in the Checkpointing Directory field. By

default, the current working directory is used. In addition, you can specify a numerical value for the frequency

of automatic checkpointing in the Automatic Checkpoint with Setting of Period field.

For more information, see Setting Job Scheduler Options When Running on Remote Linux Ma-

chines (p. ) or Part I: Running Fluent Under LSF.

Select Use SGE to use the SGE load management system.You can choose to set values for the SGE

qmaster, as well as the SGE queue, or the SGE pe. Alternatively, you can select Use SGE settings check

box and specify the location and name of the SGE configuration file.

chines (p. ) or Part III: Running Fluent Under SGE.

Select Use PBSPro to use the PBS Professional load management system.You can choose to set the value

for PBS Submission Host to specify the PBS Professional submission host name for submitting the job, if

the machine you are using to run the launcher cannot submit jobs to PBS Professional.

chines (p. ) or Part II: Running Fluent Under PBS Professional.

If you experience poor graphics performance when using a job scheduler in Linux, you may be able

to improve performance by changing the machine on which Cortex (the process that manages the

graphical user interface and graphics) is running. The Graphics Display Machine list provides the

Select First Allocated Node if you want Cortex to run on the same machine as that used for compute node

.

Note that it is possible to enable a job-scheduler-supported native remote node access mechanism

in Linux when the graphics display machine is set to First Allocated Node. To do so, you must use

the SCHEDULER_TIGHT_COUPLING= environment variable. For details about the MPI / job

scheduler combinations that are supported for this tight coupling, see Running Fluent Using a Load

Manager.

Select Current Machine if you want Cortex to run on the same machine used to start Fluent Launcher.

Select Specify Machine if you want Cortex to run on a specified machine, which you select from the drop-

down list below.

Important

(Exceed onDemand Only) If you select the Current Machine or Specify Machine, you must

also set the CORTEX_PRE=ssrun environment variable to specify the server side rendering

to ensure accelerated graphics performance.

For example: CORTEX_PRE=/opt/Exceed_connection_server_13.8_64/bin/ss-

run.

For Windows, you also have the ability to run in batch mode (using the Run in Batch Mode check

box) when you provide a journal file (designated in the General Options tab) that exits ANSYS Fluent

at the end of the run.

For machines running Microsoft HPC Pack  or newer, you also have the following options to

choose from:

Job Template allows you to create a custom submission policy to define the job parameters for an

application.The cluster administrator can use job templates to manage job submission and optimize

cluster usage.

Node Group allows you to specify a collection of nodes. Cluster administrators can create groups and

assign nodes to one or more groups.

Processor Unit allows you to choose the following:

– Core refers to a single computing unit in a machine. For example, a quad-core processor has  cores.

– Socket refers to a set of tightly integrated cores as on a single chip. Machines often have  or more

sockets, each socket with multiple cores. A dual CPU, hexcore processor, for example, having a total

of  cores.

– Node refers to a named host, that is, a single machine used as part of a cluster.Typical clusters

range from a few to tens, hundreds, or sometimes thousands of machines.

The Remote tab allows you to specify settings for running ANSYS Fluent parallel simulations on Linux

clusters, via the Windows interface.

You can run simulations on Linux machines, either in serial or on parallel Linux clusters, via the Windows

interface. To access remote -bit Linux clusters for your parallel calculation, select the Parallel (Local

Machine) option under Processing Options (for details, see Setting Parallel Options in Fluent

Launcher (p. ) in the Getting Started Guide), then enable Use Remote Linux Nodes, which appears

under Options. The Remote tab in Fluent Launcher will become available, where you can specify the

remote ANSYS Fluent Linux installation root path in the Remote Fluent Root Path field. The Remote

Working Directory field allows you to specify a working directory for the remote Linux nodes, other

than the default temp directory.

Select one of the following Remote Spawn Commands to connect to the remote node:

RSH will use RSH to spawn nodes from the local Windows machine to the Linux head node as well as from

the Linux head node to the compute nodes. If you want the Linux cluster to use SSH, then you must set

the FLUENT_NO_REMOTE_RSH to .You also must set up password-less access.

SSH (the default) will use SSH to spawn nodes from the local Windows machine to the Linux head node

as well as from the Linux head node to the compute nodes.To use SSH with ANSYS Fluent, you must set

up password-less SSH access. If you want the Linux cluster to use RSH, then you must set the FLUENT_NO_RE-

MOTE_SSH to . For more information about setting up SSH without a password, see www.debian-admin-

istration.org/articles/.

Other allows you to provide other compatible remote shell commands.

Enable the Use Remote Cluster Head Node field and specify the remote node to which ANSYS Fluent

will connect for spawning (for example, via rsh or ssh). If this is not provided, then ANSYS Fluent

will try to use the first machine in the machine file. If SGE is chosen as the job scheduler, then the SGE

qmaster will serve the same purpose. If PBS Professional is chosen as the job scheduler, then the host

specified here should be the PBS Professional submission host.

In addition to using the settings in the Remote tab in Fluent Launcher, the following command line

options are also available when starting ANSYS Fluent from the command line:

nodepath=path

is the path on the remote machine where ANSYS Fluent is installed.

node0=machine name

is the machine from which to launch other nodes.

nodehomedir=directory

is the directory that becomes the current working directory for all the nodes. Additionally, this will be

used as a scratch area for temporary files that are created on the nodes.

rsh=remote shell command

is the command that will be used to launch executables remotely.This option defaults to ssh.exe but

can point to any equivalent program.The form of this command should be that it should not wait for

additional inputs such as passwords. For example, if you install SSH, and try to launch in mixed mode

using ssh, the launch may fail unless you have set up a login for SSH without a password. For more in-

formation about setting up SSH without a password, see www.debian-administration.org/articles/.

As there are known issues with launching ANSYS Fluent in mixed Windows/Linux mode from cygwin,

it is recommended that you use the command prompt (cmd.exe).

When working with mixed Linux and Windows runs that employ user-defined functions (UDFs), note

The file that you have opened for reading / writing on the host machine will not be available on remote

nodes and vice-versa.You may therefore have to transfer data present on the nodes to the host and write

it from host, (or distribute the data from the host to the nodes after reading the data from the host).

The loading of multiple UDF libraries into the same session is not supported. As a workaround, you can

compile multiple UDF files into same UDF library.

.... Setting Job Scheduler Options When Running on Remote Linux Machines

By selecting the Use Remote Linux Nodes option and the Use Job Scheduler option in Fluent

Launcher, you can set job scheduler options for the remote Linux machines you are accessing for

your CFD analysis.

When these options are enabled in Fluent Launcher, you can use the Scheduler tab to set parameters

for either LSF, SGE, or PBS Professional job schedulers. You can learn more about each of the schedulers

by referring to the Load Management Documentation.

The following list describes the various controls that are available in the Scheduler tab:

Use LSF

allows you to use the LSF job scheduler.

LSF queue

allows you to specify a job queue and enter the queue name in the field.

Use Checkpointing

allows you to use checkpointing with LSF. By default, the checkpointing directory will be the current

working directory; however, you have the option of enabling Checkpointing Directory.

Checkpointing Directory

allows you to specify a checkpointing directory that is different from the current working directory.

Automatic Checkpoint with Setting of Period

allows you to specify that the checkpointing is done automatically at a set time interval. Enter the

period (in minutes) in the field, otherwise checkpointing will not occur unless you call the bchkpnt

command.

Use SGE

allows you to use the SGE job scheduler.

SGE qmaster

is the machine in the SGE job submission host list. SGE will allow the SGE qmaster node to summon

jobs. By default, localhost is specified for SGE qmaster. Note that the

button allows you to

check the job status.

SGE queue

is the queue where you want to submit your ANSYS Fluent jobs. Note that you can use the

button to contact the SGE qmaster for a list of queues. Leave this field blank if you want to use the

default queue.

SGE pe

is the parallel environment where you want to submit your ANSYS Fluent jobs.The parallel environ-

ment must be defined by an administrator. For more information about creating a parallel environ-

ment, refer to the SGE documentation. Leave this field blank if you want to use the default parallel

Use PBSPro

allows you to use the PBS Professional job scheduler.

Important

While running on remote Linux machines using any one of the Job Scheduler options, if

the submitted job is in the job queue because of unavailable requested resources, then

the ANSYS Fluent graphical user interface will remain open until resources are available

and the job starts running.

Note

If you experience poor graphics performance when using a job scheduler in Linux, you

may be able to improve performance by specifying that Cortex run on a specified machine

when you start Fluent. This can be done by using the -gui_machine=<hostname>

and -scheduler=<scheduler> command line options (see Graphics Options (p. )

and Scheduler Options (p. )), or by selecting Specify Machine from the Graphics Display

Machine list in the Scheduler tab of Fluent Launcher.

Note

The SCHEDULER_TIGHT_COUPLING= environment variable is not supported when

running on remote Linux machines.

You can run ANSYS Fluent on a Windows system using either the graphical user interface (for details,

see Starting Parallel ANSYS Fluent Using Fluent Launcher (p. )) or command line options (for details,

see Starting Parallel ANSYS Fluent on a Windows System Using Command Line Options (p. )).

Important

See the separate installation instructions for more information about installing parallel ANSYS

Fluent for Windows. The startup instructions below assume that you have properly set up

the necessary software, based on the appropriate installation instructions.

... Starting Parallel ANSYS Fluent on a Windows System Using Command Line Options

... Starting Parallel ANSYS Fluent on a Windows System Using Command

Line Options

To start the parallel version of ANSYS Fluent using command line options, you can use the following

syntax in a Command Prompt window:

fluent version -t nprocs [-gpgpu= ngpgpus ] [-p interconnect ] [-mpi= mpi_type ] [-cnf=

hosts ]

where

version must be replaced by the version of ANSYS Fluent you want to run (2d, 3d, 2ddp, or 3ddp).

hosts ]

where

-t nprocs specifies the number of processes to use.When the -cnf option is present, the hosts argument

is used to determine which machines to use for the parallel job. For example, if there are  machines listed

in the hosts file and you want to run a job with  processes, set nprocs to  (that is, -t4) and ANSYS Fluent

will use the first  machines listed in the hosts file. Note that this does not apply to the Compute Cluster

Server (CCS). If the -gpgpu option is used, nprocs must be chosen such that the number of solver processes

per machine is equal on all machines.

-p interconnect (optional) specifies the type of interconnect.The ethernet interconnect is used by default

if the option is not explicitly specified. See Table . : Supported Interconnects for the Windows Plat-

form (p. ), Table . : Available MPIs for Windows Platforms (p. ), and Table . : Supported MPIs for

Windows Architectures (Per Interconnect) (p. ) for more information.

-mpi= mpi_type (optional) specifies the MPI implementation. If the option is not specified, the default MPI

for the given interconnect (IBM MPI) will be used (the use of the default MPI is recommended).The available

MPIs for Windows are shown in Table . : Available MPIs for Windows Platforms (p. ).

-cnf= hosts (optional) specifies the hosts file, which contains a list of the machines on which you want to

run the parallel job; if this option is not used, then the session will run on the local machine. If the hosts

file is not located in the folder where you are typing the startup command, you must supply the full path-

name to the file.

You can use a plain text editor such as Notepad to create the hosts file. The only restriction on the

filename is that there should be no spaces in it. For example, hosts.txt is an acceptable hosts

file name, but my hosts.txt is not.

Your hosts file (for example, hosts.txt) might contain the following entries:

machine1

machine2

Important

The last entry must be followed by a blank line.

If a machine in the network is a multiprocessor, you can list it more than once. For example, if ma-

chine1 has  CPUs, then, to take advantage of both CPUs (and similarly for multicore machines),

the hosts.txt file should list machine1 twice:

machine1

machine1

machine2

equal as possible. You can control the per machine block allocation size using the machine X : Y

convention in the hosts specification, where Y is the process block count for machine X. The process

assignment will cycle through the machine list until all processes are allocated in specified blocks.

A fully round-robin assignment of processes can be achieved by setting the machine block allocation

sizes to  (for example, machine1:, machine2:, and so on).

Starting Parallel ANSYS Fluent on a Windows System

-gpgpu= ngpgpus specifies the number of GPGPUs per machine to use for AMG execution. Note that when

this option is used, the number of solver process per machine must be equal on all machines and ngpgpus

must be chosen such that the number of solver processes per machine is an integer multiple of ngpgpus.

That is, for nprocs solver processes running on M machines using ngpgpus GPGPUS per machine:

See Using General Purpose Graphics Processing Units (GPGPUs) With the Algebraic Multigrid (AMG) Solv-

er (p. ) for more information about using GPGPU acceleration.

For example, the full command line to start a 3D parallel job on the first  machines listed in a hosts

file called hosts.txt is as follows:

fluent 3d -t4 -cnf=hosts.txt

As another example, the full command line to start a 3D symmetrical multiprocessing (SMP) parallel

job on  machines is as follows:

fluent 3d -t4

In either case, the default communication library (IBM MPI), and the default interconnect (automatically

selected by the MPI used, or ethernet) will be used since these options are not specified.

The first time that you try to run ANSYS Fluent in parallel, you will be prompted for information about

the current Windows account.

The supported interconnects for dedicated parallel win64 Windows machines, the associated MPIs

for them, and the corresponding syntax are listed in Table . : Supported Interconnects for the Windows

Platform (p. ) - Table . : Supported MPIs for Windows Architectures (Per Interconnect) (p. ).

Table . : Supported Interconnects for the Windows Platform

Interconnects

Architecture

Processor

Platform

ethernet (default), infiniband

win64

bit

Windows

Table . : Available MPIs for Windows Platforms

Notes

Communication Library

Syntax (flag)

MPI

(), (), ()

IBM MPI

mpi=ibmmpi

ibmmpi

(), ()

mpi=msmpi

msmpi

(), (), ()

Intel MPI

mpi=intel

intel

() Used with Shared Memory Machine (SHM) where the memory is shared between the processors

ibmmpi

(), ()

mpi=msmpi

msmpi

(), (), ()

Intel MPI

mpi=intel

intel

on a single machine.

() Used with Distributed Memory Machine (DMM) where each processor has its own memory associated

with it.

() IBM Platform MPI Community Edition is installed with Fluent, which is limited to  processes

without an additional license. Refer to IBM Platform MPI with High (>) Process Count for details.

() Used with a job scheduler to run on a Windows high performance computing server (HPC).

() By default, the Intel MPI may fail when mixing hardware for compute nodes. As a workaround, you

can use the following environment setting:

Table . : Supported MPIs for Windows Architectures (Per Interconnect)

Infiniband

Ethernet

msmpi

ibmmpi (default), intel, msmpi

win64

.... Starting Parallel ANSYS Fluent with the Microsoft Job Scheduler

The Microsoft Job Scheduler allows you to manage multiple jobs and tasks, allocate machine resources,

send tasks to compute nodes, and monitor jobs, tasks, and compute nodes.

The Windows Server operating systems include a compute cluster server (CCS) and a high performance

computing server (HPC) that combines the Microsoft MPI type (msmpi) with the Microsoft Job

Scheduler. ANSYS Fluent provides a means of using the Microsoft Job Scheduler using the following

flag in the parallel command:

ccp head-node-name

where -ccp indicates the use of the compute cluster server package, and head-node-name indicates

the name of the head node of the machine cluster.

For example, if you want to use the Microsoft Job Scheduler to run a 3D model on  nodes, the cor-

responding command syntax would be:

fluent 3d -t2 -ccp head-node-name

Important

Both the IBM MPI type (ibmmpi) and the Intel MPI (intel) are not supported with the

Microsoft Job Scheduler.

Note

When using Microsoft Job Scheduler, the best interconnect is automatically selected by

MS-MPI.

Though the usage described previously is recommended as an initial starting point for running ANSYS

Fluent with the Microsoft Job Scheduler, there are further options provided to meet your specific

needs. ANSYS Fluent allows you to do any of the following with the Microsoft Job Scheduler:

Request resources from the Microsoft Job Scheduler first, before you launch ANSYS Fluent.

This is done by first submitting a job that will run until canceled, as shown in the following example:

job new/scheduler: head-node-name /numprocessors: /rununtilcanceled:true

This example requests a -node resource on a cluster named head-node-name. You will see that a

job is created with the job ID job-id:

job submit/scheduler:  head-node-name /id:  job-id

Then check if the resources have been allocated:

job view job-id /scheduler: head-node-name

If the resources are ready, you can start ANSYS Fluent using the job ID:

fluent 3d -t2 -ccp head-node-name -jobid= job-id

This job will be reusable until you decide to cancel it, at which point you must enter the following:

job cancel job-id /scheduler: head-node-name

Have ANSYS Fluent submit a CCS job, but delay the launching of ANSYS Fluent until the actual resources

are allocated.

This is done by specifying the job ID as -, as shown in the following example:

fluent 3d -t2 -ccp head-node-name -jobid=-

If you want to stop the job application, click the Cancel button. ANSYS Fluent will prompt you for

confirmation, and then clean up the pending job and exit.

Run your job using XML template files.

This is done by first creating an XML template file, such as shown in the following example:

<?xml version="." encoding="utf-"?>

<Job

xmlns:m:xsi="http://www.w3.org//XMLSchema-instance"

xmlns:m:xsd="http://www.w3.org//XMLSchema"

SoftwareLicense=""

MaximumNumberOfProcessors=""

MinimumNumberOfProcessors=""

Runtime="Infinite"

IsExclusive="true"

Priority="Normal"

Name="Name_of_job"

Project="Fluent runs"

RunUntilCanceled="false">

<Tasks xmlns:m="http://www.microsoft.com/ComputeCluster/">

<Task

Depend=""

WorkDirectory="\\file-server\home\user"

Stdout="fluent-case.%CCP_JOBID%.out"

Stderr="fluent-case.%CCP_JOBID%.err"

Name="My Task"

CommandLine="\\head-node\fluent-sharename\win64\fluent.exe 3d -i bsi.jou -t4"

IsRerunnable="false"

Runtime="Infinite">

</Task>

</Tasks>

</Job>

where fluent-sharename is the name of the shared directory pointing to where ANSYS Fluent

is installed (for example, C:\Program Files\ANSYS Inc\v195\fluent).

Important

Note that you must create a journal file that exits ANSYS Fluent at the end of the run,

and refer to it using the -i flag in your XML template file (bs1.jou in the previous

example).

Important

example).

After you have saved the file and given it a name (for example, job1.xml), you can submit the

job as shown:

job submit /jobfile:job1.xml

Run the job in batch mode without displaying the ANSYS Fluent graphical user interface.

The following is an example of such a batch mode job:

job submit /scheduler: head-node-name

/numprocessors: /workdir:\\file-server\home\user\

\\head-node\fluent-sharename\ntbin\win64\fluent.exe 3d -t2 -i bs1.jou

Important

– Note that you must create a journal file that exits ANSYS Fluent at the end of the run, and

refer to it using the -i flag in your batch mode job submission (bs1.jou in the previous

example).

– You can start ANSYS Fluent jobs from any machine on which is installed either the full CCP

or the CCP client tools, but note that all the machines must have the same version installed.

You can run ANSYS Fluent on a Linux system using either the graphical user interface (for details, see

Starting Parallel ANSYS Fluent Using Fluent Launcher (p. )) or command line options (for details, see

Starting Parallel ANSYS Fluent on a Linux System Using Command Line Options (p. ) and Setting Up

Your Remote Shell and Secure Shell Clients (p. )).

Important

On some clusters without accelerated graphics, Fluent may not accept keyboard inputs. If

you encounter this behavior, set the QT_XKB_CONFIG_ROOT environment variable equal

Important

to /usr/share/X11/xkb.

Starting Parallel ANSYS Fluent on a Linux System

... Starting Parallel ANSYS Fluent on a Linux System Using Command Line Options

... Setting Up Your Remote Shell and Secure Shell Clients

... Starting Parallel ANSYS Fluent on a Linux System Using Command

syntax in a command prompt window:

hosts ]

where

in the hosts file and you want to run a job with  processes, set nprocs to  (that is, -t5) and ANSYS Fluent

will use the first  machines listed in the hosts file. Note that if the -gpgpu option is used, nprocs must be

chosen such that the number of solver processes per machine is equal on all machines.

-p interconnect (optional) specifies the type of interconnect.The auto-select interconnect is used by

default so that the best available interconnect is used if the option is not explicitly specified. See

Table . : Supported Interconnects for Linux Platforms (Per Platform) (p. ), Table . : Available MPIs

for Linux Platforms (p. ), and Table . : Supported MPIs for Linux Architectures (Per Interconnect) (p. )

for more information.

-mpi= mpi_type (optional) specifies the type of MPI. If the option is not specified, the default MPI for the

given interconnect will be used (the use of the default MPI is recommended).The available MPIs for Linux

are shown in Table . : Available MPIs for Linux Platforms (p. ).

file is not located in the directory where you are typing the startup command, you must supply the full

pathname to the file.

You can use a plain text editor to create the hosts file. The only restriction on the filename is that

there should be no spaces in it. For example, hosts.txt is an acceptable hosts file name, but my

hosts.txt is not.

machine1

machine2

chine1 has  CPUs, then, to take advantage of both CPUs, the hosts.txt file should list machine1

twice:

machine1

machine1

machine2

As an alternative to a hosts file, you can simply type the names of the machines in a list separated

by commas, as shown in the following example: -cnf=machine1,machine1,machine2.

For example, to use the Infiniband interconnect, and to start the 3D solver with  compute nodes on

the machines defined in the text file called fluent.hosts, you can enter the following in the com-

mand prompt:

fluent 3d -t4 -pinfiniband -cnf=fluent.hosts

Note that if the optional -cnf= hosts is specified, a compute node will be spawned on each machine

listed in the file hosts.

Also, ANSYS Fluent provides a fault-tolerance feature on Infiniband Linux clusters running OFED. To

invoke this feature, use the command line flag -pinfiniband.ofedft (or -pib.ofedft), which

enables transparent port fail-over and high-availability features using the IBM MPI. Note that while the

simulations proceed more robustly with this option, there may be some degradation in performance.

During startup, ANSYS Fluent will create very small text files in the /tmp area. If you would like to

specify a different location for these files, set the following environment variable: export FL_TMPDIR=

The supported interconnects for parallel Linux machines are listed below (Table . : Supported Inter-

connects for Linux Platforms (Per Platform) (p. ), Table . : Available MPIs for Linux Platforms (p. ),

and Table . : Supported MPIs for Linux Architectures (Per Interconnect) (p. )), along with their as-

sociated communication libraries, the corresponding syntax,

Table . : Supported Interconnects for Linux Platforms (Per Platform)

Interconnects/Systems*

Processor

Platform

ethernet, infiniband, crayx

lnamd64

bit

Linux

(*) Node processes on the same machine communicate by shared memory. ANSYS Fluent lets the MPI

autoselect the best interconnect available on the system. Users can specify an interconnect to override

that selection. Ethernet is the fallback choice.

Table . : Available MPIs for Linux Platforms

Notes

MPI

General purpose for SMPs

and clusters

()

IBM MPI

ibmmpi

Intel MPI

mpi=intel

intel

Open source MPI-

implementation. For both

SMPs and clusters.

Open MPI

mpi=openmpi

()

IBM MPI

ibmmpi

Intel MPI

mpi=intel

intel

Open MPI

openmpi

Only available on Cray

systems.

mpi=cray

cray

Table . : Supported MPIs for Linux Architectures (Per Interconnect)

Omni-Path**

Proprietary

Systems

Ethernet

ibmmpi (default)

and intel

cray*

ibmmpi (default),

intel, and

openmpi

intel, and

openmpi

lnamd64

(*) Using the Cray platform, the Extreme Scalability Mode (ESM) option is used by default, employing

the native Cray MPI (MPT) library for parallel communication. Optionally, you can use the Cluster

Compatibility Mode (CCM) mode, in which the standard IBM MPI library is used for parallel communic-

ation. For simulations with high core counts (for example, above  cores), the ESM mode is recom-

mended for better performance. Note that when using MPT version . and higher (up to, but not in-

cluding . ), you must set the following environment variable: export FLUENT_USE_CRAY_MPT5=.

(**) For Intel Omni-Path architecture, Omni-Path software . or higher is recommended, and Intel

MPI is preferred.

(Linux Only) To enable a job-scheduler-supported native remote node access mechanism, you can use

the -scheduler_tight_coupling command line option. For details about the MPI / job scheduler

combinations that are supported for this tight coupling, see Running Fluent Using a Load Manager.

For cluster computing on Linux systems, most parallel versions of ANSYS Fluent will require the user

account set up such that you can connect to all nodes on the cluster (using either the remote shell

(rsh) client or the secure shell (ssh) client) without having to enter a password each time for each

machine.

Provided that the appropriate server daemons (either rshd or sshd) are running, this section briefly

describes how you can configure your system in order to use ANSYS Fluent for parallel computing.

.... Configuring the rsh Client

The remote shell client (rsh), is widely deployed and used. It is generally easy to configure, and in-

volves adding all the machine names, each on a single line, to the .rhosts file in your home directory.

If you refer to the machine you are currently logged on as the ‘client’, and if you refer to the remote

machine to which you seek password-less login as the ‘server’, then on the server, you can add the

name of your client machine to the .rhosts file. The name could be a local name or a fully qualified

name with the domain suffix. Similarly, you can add other clients from which you require similar access

to this server. These machines are then “trusted” and remote access is allowed without the further

need for a password. This setup assumes you have the same user ID on all the machines. Otherwise,

each line in the .rhosts file must contain the machine name as well as the user ID for the client

that you want access to. Refer to your system documentation for further usage options.

Note that for security purposes, the .rhosts file must be readable only by the user.

.... Configuring the ssh Client

The secure shell client (ssh), is a more secure alternative than rsh and is also used widely. Depending

on the specific protocol and the version deployed, configuration involves a few steps. SSH1 and

SSH2 are two current protocols. OpenSSH is an open implementation of the SSH2 protocol and is

backwards compatible with the SSH1 protocol. To add a client machine, with respect to user config-

uration, the following steps are involved:

. Generate a public-private key pair using ssh-keygen (or using a graphical user interface client). For

example:

% ssh-keygen -t dsa

where it creates a Digital Signature Authority (DSA) type key pair.

. Place your public key on the remote host.

For SSH1, insert the contents of the client (~/.ssh/identity.pub) into the server

(~/.ssh/authorized_keys).

For SSH2, insert the contents of the client (~/.ssh/id_dsa.pub) into the server (~/.ssh/au-

thorized_keys2).

The client machine is now added to the access list and you are no longer required to type in a password

each time. For additional information, consult your system administrator or refer to your system

Information about mesh partitioning and load balancing is provided in the following sections:

... Overview of Mesh Partitioning

... Partitioning the Mesh Automatically

... Partitioning the Mesh Manually and Balancing the Load

Mesh Partitioning and Load Balancing

... Using the Partitioning and Load Balancing Dialog Box

... Mesh Partitioning Methods

... Checking the Partitions

... Load Distribution

When you use the parallel solver in ANSYS Fluent, you must partition or subdivide the mesh into

groups of cells that can be solved on separate processors (see Figure . : Partitioning the Mesh (p. )).

You can either use the automatic partitioning algorithms when reading an unpartitioned mesh into

the parallel solver (recommended approach, described in Partitioning the Mesh Automatically (p. )),

or perform the partitioning yourself in the serial solver or after reading a mesh into the parallel solver

(as described in Partitioning the Mesh Manually and Balancing the Load (p. )). In either case, the

available partitioning methods are those described in Mesh Partitioning Methods (p. ). You can

partition the mesh before or after you set up the problem (by defining models, boundary conditions,

and so on).

Note that the relative distribution of cells among compute nodes will be maintained during mesh ad-

aption, so manual repartitioning after adaption is not required. For details, see Load Distribution (p. ).

If you use the serial solver to set up the problem before partitioning, the machine on which you perform

this task must have enough memory to read in the mesh. If your mesh is too large to be read into the

serial solver, you can read the unpartitioned mesh directly into the parallel solver (using the memory

available in all the defined hosts) and have it automatically partitioned. In this case you will set up the

problem after an initial partition has been made. You will then be able to manually repartition the

case if necessary. See Partitioning the Mesh Automatically (p. ) and Partitioning the Mesh Manually

and Balancing the Load (p. ) for additional details and limitations, and Checking the Partitions (p. )

for details about checking the partitions.

Figure . : Partitioning the Mesh

For automatic mesh partitioning, you can select the partition method and other options for creating

the mesh partitions before reading a case file into the parallel version of the solver. For some of the

methods, you can perform pretesting to ensure that the best possible partition is performed. See Mesh

Partitioning Methods (p. ) for information about the partitioning methods available in ANSYS Fluent.

Note

Architecturally aware partitioning (see Partitioning (p. )) is performed automatically when

the case file is read. If the maximum inter-machine communication is reduced by more than

%, the new partition mapping will be applied, and a message is displayed in the console,

for example:

inter-node communication reduction by architecture-aware remap-

ping: %

While the message indicates actual point-to-point network traffic reduction, solver compu-

tational performance improvement may be somewhat less, and depends on the case and

the system network configuration.

The procedure for partitioning automatically in the parallel solver is as follows:

. (optional) Set the partitioning parameters in the Auto Partition Mesh dialog box (Figure . :The Auto

Partition Mesh Dialog Box (p. )).

Parallel → General → Auto Partition...

Figure . : The Auto Partition Mesh Dialog Box

If you are reading in a mesh file or a case file for which no partition information is available, and

you keep the Case File option turned on, ANSYS Fluent will partition the mesh using the method

displayed in the Method drop-down list.

If you want to specify the partitioning method and associated options yourself, the procedure is

a.

Turn off the Case File option.The other options in the dialog box will become available.

b. Select the partition method in the Method drop-down list.The choices are the techniques described

in Partition Methods (p. ).

c.

You can choose to independently apply partitioning to each cell zone, or you can allow partitions

to cross zone boundaries using the Across Zones check button (which is enabled by default).

It is recommended that you leave this option enabled, as otherwise the resulting partitions may

be too granularized, which can compromise performance. Note that disabling this option has

no effect when you have selected Metis for the Method.

d. If you have chosen the Principal Axes or Cartesian Axes method, you can improve the partitioning

by enabling the automatic testing of the different bisection directions before the actual partitioning

occurs.To use pretesting, turn on the Pre-Test option. Pretesting is described in Pretesting (p. ).

If you have a case file where you have already partitioned the mesh, and the number of partitions

divides evenly into the number of compute nodes, you can keep the default selection of Case File

in the Auto Partition Mesh dialog box. This instructs ANSYS Fluent to use the partitions in the

case file.

.... Reporting During Auto Partitioning

As the mesh is automatically partitioned, some information about the partitioning process will be

displayed in the console. If you want additional information, you can display a report from the Parti-

tioning and Load Balancing dialog box after the partitioning is completed.

Parallel → General → Partition/Load Balance...

When you click the Print Active Partitions or Print Stored Partitions button in the Partitioning

and Load Balancing dialog box, ANSYS Fluent will display the partition ID, number of cells, faces,

and interfaces, and the ratio of interfaces to faces for each active or stored partition in the console.

In addition, it will display the minimum and maximum cell, face, interface, and face-ratio variations.

For details, see Interpreting Partition Statistics (p. ). You can examine the partitions graphically by

following the directions in Checking the Partitions (p. ).

Automatic partitioning in the parallel solver (described in Partitioning the Mesh Automatically (p. ))

is the recommended approach to mesh partitioning, but it is also possible to partition the mesh

manually in either the serial solver or the parallel solver. After automatic or manual partitioning, you

will be able to inspect the partitions created (for details, see Checking the Partitions (p. )) and op-

tionally repartition the mesh, if necessary. Again, you can do so within the serial or the parallel solver,

using the Partitioning and Load Balancing dialog box. A partitioned mesh may also be used in the

serial solver without any loss in performance.

.... Guidelines for Partitioning the Mesh

The following steps are recommended for partitioning a mesh manually:

. Partition the mesh using the default method (Metis). Metis will generally produce the best quality

partitions for most problems and no further user intervention should be necessary. Note that the

Cartesian Axes method can be a reasonable alternative with less memory overhead.

. Examine the partition statistics, which are described in Interpreting Partition Statistics (p. ). Your

aim is to minimize the Maximum value of the Partition boundary face count ratio,

while maintaining a balanced load. For a given mesh, the Mean cell count deviation is

a measure of the maximum load imbalance for a method. If the statistics are not satisfactory for

a problem, you can try one of the other partitioning methods.

Instructions for manual partitioning are provided below.

.... Partitioning

In order to partition the mesh, you must select the partition method for creating the mesh partitions,

set the number of partitions, select the zones and/or registers, and choose the optimizations to be

used. For some methods, you can also perform pretesting to ensure that the best possible partition

is performed. Once you have set all the parameters in the Partitioning and Load Balancing dialog

box to your satisfaction, click the Partition button to subdivide the mesh into the selected number

of partitions using the prescribed method and optimization(s). For recommended partitioning strategies

see Guidelines for Partitioning the Mesh (p. ).

You can set the relevant inputs in the Partitioning and Load Balancing dialog box (Figure . : The

Partitioning and Load Balancing Dialog Box (p. )) in the following manner:

Figure . : The Partitioning and Load Balancing Dialog Box

. Select the Method from the drop-down list.The choices are described in Partition Methods (p. ).

. In the Options tab

a.

Set the desired number of mesh partitions in the Number of Partitions field.You can use the counter

arrows to increase or decrease the value, instead of typing in the box.The number of mesh partitions

must be an integer number that is divisible by the number of processors available for parallel com-

puting.

b. Set the Reporting Verbosity.This allows you to control what is displayed in the console. For details,

see Reporting During Partitioning (p. ).

c.

You can choose to independently apply partitioning to each cell zone, or you can allow parti-

tions to cross zone boundaries using the Across Zones check button (which is enabled by

default). It is recommended that you leave this option enabled, as otherwise the resulting

partitions may be too granularized, which can compromise performance. Note that disabling

this option has no effect when you have selected Metis for the Method.

d. If you are using the Metis method, you have the option of enabling Laplace Smoothing.This option

can be used to prevent partition boundaries from passing through areas of high aspect ratio cells.

This can improve convergence in dynamic mesh cases and other cases with regions of highly stretched

cells. After enabling Laplace Smoothing, you can specify the Cutoff Aspect Ratio.The Cutoff Aspect

Ratio corresponds roughly to the maximum aspect ratio allowable along a partition boundary.

e. Select the Reordering Method for partitions to optimize parallel performance:

Architecture Aware:This is the default option and it accounts for the system architecture and

network topology in remapping the partitions to the processors.

Reverse Cuthill-McKee:This option minimizes the bandwidth of the compute-node connectivity

matrix (the maximum distance between two connected processes) without incorporating the

system architecture.

The reordering methods are parallel performance tuning options. After the case is initially

partitioned for parallel processing, the partition reordering step will remap the partitions in a

more optimal way to improve parallel performance.

Important

The Architecture-aware reordering method is not applicable when only a single

machine is used for the simulation.

After initially loading the case into a parallel session, you can click the Reorder button to reorder

the partitions. The necessary algorithms are executed and ANSYS Fluent will report if it can

find a more optimal mapping for the partitions, as well as the potential improvement in inter-

machine communications. If the reported improvement is significant (say, more than %), then

you can click the Use Stored Partitions button to use the new partition mapping. This will

generally entail large data transfers amongst all the processes, and another reliable method

to use the new partitions would be to write out a case file and load it back in to a new parallel

session. The process is similar to re-partitioning with a new partitioning method, for example.

Note that sometimes, depending on the cluster configuration and initial case partitioning, and

if the partitions have already been reordered, no improvement is possible, and this will be re-

ported in the console after clicking the Reorder button. You can simply continue in this case,

and there will be no effect on the simulation. Also, note that partition reordering is specific

to the current parallel configuration and should be repeated if the number of machines used

changes during subsequent computations.

. In the Optimization tab

a.

You can enable and control the desired optimization methods (described in Optimizations (p. )).

You can enable the Merge and Smooth schemes by enabling the check button next to each one.

For each scheme, you can also set the number of Iterations. Each optimization scheme will be applied

until appropriate criteria are met, or the maximum number of iterations has been executed. If the

Iterations counter is set to , the optimization scheme will be applied until completion, with no

limit on maximum number of iterations.

b. Choosing the Principal Axes or Cartesian Axes method, you can improve the partitioning by enabling

the automatic testing of the different bisection directions before the actual partitioning occurs.To

use pretesting, enable the Pre-Test option. Pretesting is described in Pretesting (p. ).

. In the Zones and/or Registers lists, select the zone(s) and/or register(s) for which you want to partition.

For most cases, you will select all Zones (the default) to partition the entire domain. See below for details.

. You can assign selected Zones and/or Registers to a specific partition ID by entering a value for the Set

Selected Zones and Registers to Partition ID. For example, if the Number of partitions for your mesh

is , then you can only use IDs of  or . If you have three partitions, then you can enter IDs of , , or

.This can be useful in situations where the gradient at a region is known to be high. In such cases, you

can mark the region or zone and set the marked cells to one of the partition IDs, thereby preventing the

partition from going through that region.This in turn will facilitate convergence.This is also useful in

cases where mesh manipulation tools are not available in parallel. In this case, you can assign the related

cells to a particular ID so that the mesh manipulation tools are now functional.

If you are running the parallel solver, and you have marked your region and assigned an ID to

the selected Zones and/or Registers, click the Use Stored Partitions button to make the new

partitions valid.

Refer to the example described later in this section for a demonstration of how selected registers

are assigned to a partition (Example of Setting Selected Cell Registers to Specified Partition

IDs (p. )).

. In the Weighting tab (Figure . : The Weighting Tab in the Partitioning and Load Balancing

Dialog Box (p. )), you can set the appropriate weights prior to partitioning the mesh, to improve

load balancing and overall performance. You can control weights for cells, solid cell zones, VOF,

DPM, and ISAT table lookup. You can rely on ANSYS Fluent timers to set the weight scaling and

optionally modify it (by enabling the User Specified option); alternatively, you can use model-

weighted partitioning, so that Fluent automatically calculates the weighting based on the cell

count and the models and attributes used as weights.

Figure . : The Weighting Tab in the Partitioning and Load Balancing Dialog Box

a.

Enable Faces per Cell so that the partitioning assigns a weight to each cell based on its number of

faces.This type of weighting is advantageous when the case has mixed or polyhedral cell zones. If

you enable the User Specified check box, the weight assigned to each cell will be the number of

faces plus the Additional Cell Weight you enter in the number-entry box under Value. By default

the Faces per Cell weighting is enabled with the Additional Cell Weight set to .

b. Enable Solid Zones weighting so that the partitioning takes solid cells into consideration. If

you enable the User Specified check box, you can specify a Value for the Solid Cell Weight

Ratio. This value is relative to the fluid cell weighting; typically, it should be less than , since

the calculation is usually quicker and less computationally expensive for the solid zone compared

to the fluid zone. When using model-weighted partitioning, the default value of . is appro-

priate, otherwise a larger value may be more suitable. For cases that have solid zones, the

Solid Zones weighting is enabled by default.

c.

Enable VOF weighting to allow the partitioning to consider the imbalance caused by the free surface

reconstruction with the geo-reconstruct scheme.Therefore, it is only available when using the VOF

model with geometric reconstruction.You may use the user-specified value before timers are collected,

or if you want to specify a value other than timing statistics.The specified value is the VOF proportion

of the total computational effort.

d. Enable DPM weighting to set the weight of DPM particles relative to the continuous phase. DPM

weights are valid when you have particle tracking in your simulation, where the user-specified value

is the DPM proportion of the total computational effort relative to the continuous phase. Note that

this is available only when you have injections defined. For details, see Modeling Discrete Phase (p. ).

The DPM weight takes into account the distribution of the tracking effort over the partitions

and it is available after at least one calculation step with particle tracking. Displaying Particle

Tracks does not change the weights. The computational effort is determined by the number

of DPM steps performed in each cell. This weight becomes more important when the time for

the particle tracking of particles exceeds the time for solving the flow. Enabling this option in

the Weighting tab enables the counting of the particle steps in the cells. These values are

available for contour and vector plots when using the Discrete Phase Model and DPM Steps

per Cell variable. After repartitioning, the DPM weights are reset before the next particle

tracking. It is generally preferable to partition along the dominant path of the particles in order

to minimize particles crossing partition boundaries and thereby reducing associated commu-

nication costs. However, partitioning should also consider load balance for the other models,

especially the continuous phase, and model weighting provides a means to effectively load

balance the overall simulation.

Select the Hybrid Optimization option to enable the hybrid optimization partition weighting

method for DPM. This method balances the load across machines, and, within each machine,

the hybrid parallel DPM method is used to make sure the load is balanced by multi-threading.

First, the domain is split based on the model weights of each cell and then partitioned across

a number of machines. Finally, each machine is partitioned according to the number of cores.

This allows you to have a balanced number of cells in each partition, at the same time having

a balanced number of particles on each machine, which will be further balanced by the hybrid

DPM method. This optimization option is also applicable to the discrete element method (DEM)

collision model.

e. Enable ISAT weighting to balance the load during the ISAT table lookup for the stiff-chemistry Lam-

inar, EDC or PDF Transport models.The ISAT algorithm builds an unstructured table in

species di-

mensions for storage and retrieval of the chemistry mappings. Since chemistry is usually computa-

tionally expensive, this storage/retrieval can be very time-consuming (for information about ISAT,

refer to In-Situ Adaptive Tabulation (ISAT) in the Theory Guide). Each parallel node builds its own

table, and there is no message passing to tables on other nodes. As some nodes may have more

chemical reactions than others (for example one parallel node may contain just air at a constant

temperature, in which case the ISAT table will contain only one entry and calculation will be rapid),

there may be a load imbalance.The dynamic load balancing algorithm will migrate cells from high

computational load nodes to low computational load nodes.

If you decide to specify a value, this user-specified value is the ISAT proportion of the total

computational effort.

f.

For the Metis partition method, you have the option of using model-weighted partitioning.

The objective of model-weighted partitioning is to balance the overall number of cells, as well

as the time needed for the selected models (that is, the enabled Weight Types, described

previously). This is specifically useful for cases that could potentially lead to a load imbal-

ance—for example: when using the discrete phase model, as the distribution of particles could

be different across partitions and thus cause an imbalance; or for cases with a large proportion

of solid zones, as solid zones require less processing time / expense than fluid zones.

Each model is considered as a constraint, and a base constraint is automatically introduced

for the overall number of cells. When partitioning, ANSYS Fluent will automatically calculate

the weights for these constraints, and balance each of them.

To use model-weighted partitioning, ensure that the Metis partition method is selected, and

enable the appropriate models under Weight Types in the Weighting tab; note that for VOF,

DPM, and ISAT, the associated User Specified and Value settings are not relevant). Then

make sure that the following text command is enabled (which it is by default) prior to parti-

tioning:

parallel → partition → set → model-weighted-partition

Note that you can get additional information specific to the constraints by setting the Reporting

Verbosity to  in the Options tab.

. When using the dynamic mesh model in your parallel simulations, the Partition dialog box includes

an Auto Repartition option and a Repartition Interval setting. These parallel partitioning options

are provided because ANSYS Fluent migrates cells when local remeshing and smoothing are per-

formed. Therefore, the partition interface becomes very wrinkled and the load balance may deteri-

orate. By default, the Auto Repartition option is selected, where a percentage of interface faces

and loads are automatically traced. When this option is selected, ANSYS Fluent automatically de-

termines the most appropriate repartition interval based on various simulation parameters.

Sometimes, using the Auto Repartition option provides insufficient results, therefore, the Repar-

tition Interval setting can be used. The Repartition Interval setting lets you to specify the interval

(in time steps or iterations respectively) when a repartition is enforced. When repartitioning is not

desired, you can set the Repartition Interval to zero.

Important

Note that when dynamic meshes and local remeshing is utilized, updated meshes may

be slightly different in parallel ANSYS Fluent (when compared to serial ANSYS Fluent

or when compared to a parallel solution created with a different number of compute

nodes), resulting in very small differences in the solutions.

. Click the Partition button to partition the mesh.

. Click the Use Stored Partitions button if you decide that the new partitions are better than the

previous ones (if the mesh was already partitioned). This makes the newly stored cell partitions

the active cell partitions. The active cell partition is used for the current calculation, while the

stored cell partition (the last partition performed) is used when you save a case file.

..... Example of Setting Selected Cell Registers to Specified Partition IDs

. Start ANSYS Fluent in parallel.The case in this example was partitioned across two nodes.

. Read in your case.

. Display the mesh with the Partitions option enabled in the Mesh Display dialog box (Figure . :The

Partitioned Mesh (p. )).

Figure . : The Partitioned Mesh

. Mark your cells using a region cell register (for details, see Region (p. )).This creates a cell register.

. Open the Partitioning and Load Balancing dialog box.

. Set the Set Selected Zones and Registers to Partition ID to  and click the corresponding button.

This displays the following output in the ANSYS Fluent console:

>>  Active Partitions:

----------------------------------------------------------------------

Collective Partition Statistics:      Minimum      Maximum   Total

Cell count

Mean cell count deviation             .%         .%

Partition boundary cell count

Partition boundary cell count ratio   .%         .%      .%

Face count

Mean face count deviation             -.%       .%

Partition boundary face count

Partition boundary face count ratio   .%        .%      .%

Partition neighbor count

Partition Method                      Metis

Stored Partition Count

Done.

. Click the Use Stored Partitions button to make the new partitions valid.This migrates the partitions

to the compute-nodes.The following output is then displayed in the ANSYS Fluent console:

Migrating partitions to compute-nodes.

P   Cells  I-Cells  Cell Ratio   Faces  I-Faces  Face Ratio  Neighbors

. .

. .

Collective Partition Statistics:     Minimum       Maximum      Total

. .

. .

Cell count

Mean cell count deviation            -.%        .%

Partition boundary cell count ratio  .%          .%         .%

Face count

Mean face count deviation            -.%        .%

Partition boundary face count ratio  .%          .%         .%

Partition Method                     Metis

Done.

. Display the mesh (Figure . :The Partitioned ID Set to Zero (p. )).

Figure . : The Partitioned ID Set to Zero

. This time, set the Set Selected Zones and Registers to Partition ID to  and click the corresponding

button.This displays a report in the ANSYS Fluent console.

. Click the Use Stored Partitions button to make the new partitions valid and to migrate the partitions

to the compute-nodes.

. Display the mesh (Figure . :The Partitioned ID Set to  (p. )). Notice now that the partition appears

in a different location as specified by your partition ID.

Figure . : The Partitioned ID Set to

Important

Although this example demonstrates setting selected registers to specific partition IDs in

parallel, it can be similarly applied in serial.

..... Partitioning Within Zones or Registers

The ability to restrict partitioning to cell zones or registers gives you the flexibility to apply different

partitioning strategies to subregions of a domain. For example, if your geometry consists of a cyl-

indrical plenum connected to a rectangular duct, you may want to partition the plenum using the

Cylindrical Axes method, and the duct using the Cartesian Axes method.

If the plenum and the duct are contained in two different cell zones, you can select one at a time

and perform the desired partitioning, as described in Using the Partitioning and Load Balancing

Dialog Box (p. ). If they are not in two different cell zones, you can create a cell register (basically

a list of cells) for each region using the functions that are used to mark cells for adaption. These

functions allow you to mark cells based on physical location, cell volume, gradient or isovalue of a

particular variable, and other parameters. See Adapting the Mesh (p. ) for information about

marking cells for adaption. Using Cell Registers (p. ) provides information about creating cell re-

gisters. Once you have created a cell register, you can partition within it as described in Example of

Setting Selected Cell Registers to Specified Partition IDs (p. ).

Important

Note that partitioning within zones or registers is not available when Metis is selected

as the partition Method.

For dynamic mesh applications, ANSYS Fluent stores the partition method used to partition the re-

spective zone. Therefore, if repartitioning is done, ANSYS Fluent uses the same method that was

used to partition the mesh.

..... Reporting During Partitioning

As the mesh is partitioned, information about the partitioning process will be displayed in the console.

By default, the number of partitions created, the time required for the partitioning, and the minimum

and maximum cell, face, interface, and face-ratio variations will be displayed (for details, see Inter-

preting Partition Statistics (p. )). If you increase the Reporting Verbosity to  from the default

value of , the partition method used, the partition ID, number of cells, faces, and interfaces, and

the ratio of interfaces to faces for each partition will also be displayed in the console. If you decrease

the Reporting Verbosity to , only the number of partitions created and the time required for the

partitioning will be reported.

You can request a portion of this report to be displayed again after the partitioning is completed.

When you click the Print Active Partitions or Print Stored Partitions button in the serial or parallel

solver, ANSYS Fluent will display the partition ID, number of cells, faces, and interfaces, and the ratio

of interfaces to faces for each active or stored partition in the console. In addition, it will display the

minimum and maximum cell, face, interface, and face-ratio variations. For details, see Interpreting

Partition Statistics (p. ).

Important

Recall that to make the stored cell partitions the active cell partitions you must click the

Use Stored Partitions button. The active cell partition is used for the current calculation,

while the stored cell partition (the last partition performed) is used when you save a case

file.

..... Resetting the Partition Parameters

If you change your mind about your partition parameter settings, you can easily return to the default

settings assigned by ANSYS Fluent by clicking on the Default button. When you click the Default

button, it will become the Reset button. The Reset button allows you to return to the most recently

saved settings (that is, the values that were set before you clicked on Default). After execution, the

Reset button will become the Default button again.

.... Load Balancing

A dynamic load balancing capability is available in ANSYS Fluent. The principal reason for using par-

allel processing is to reduce the turnaround time of your simulation, which may be achieved by the

following means:

Faster machines, for example, faster CPU, memory, cache, and communication bandwidth between the

CPU and memory

Faster interconnects, for example, smaller latency and larger bandwidth

Better Load balancing, for example, load is evenly distributed and CPUs are not idled during calculation

The first two evolve at the pace of computer technology, which is beyond the scope of this document.

The third item is regarding optimization of available computation power. Here we are mainly talking

about load balancing on dedicated homogeneous resources, which is often the case nowadays. If

you are not using a dedicated homogeneous resource, you may need to account for differences in

CPU speeds during partitioning by specifying a load distribution (for details, see Load Distribu-

On a dedicated homogeneous system, the key for load balancing is how to evaluate the computational

requirement of each cell. By default, ANSYS Fluent assumes that each cell requires the same compu-

tational work, but this is often not the case. For example

A hexahedral cell demands more CPU and memory than a tetrahedral cell.

A cell with particle tracking will use more time than a cell without particle tracking.

ISAT species model cells may have magnitude differences in time usage.

To balance these differences, ideally, the time used in each cell could be recorded and load balance

achieved based on these detailed timing statistics. However, this can be expensive and such low level

timings can be unreliable in any case. Instead, we identify features causing computational imbalance

and record time usage for these models in aggregate. For a more detailed description of this, refer

to Partitioning (p. ) in the discussion of the Weighting tab. In addition, the imbalance may happen

dynamically during run time, for example

The mesh may be changed by adaption or mesh movement.

In unsteady cases, particle tracking may move from one region to another region.

Dynamic load balancing has been implemented for better scalability of cases with imbalanced phys-

ical or geometrical models, thereby reducing the simulation time. The implementation considers

weights from these models scaled by CPU time usage. Load balancing for DPM, VOF, cell type (number

of faces per cell), and solid zones can be performed. In addition, cell weight based load balancing

and machine load distribution can also be specified (for details, see Load Distribution (p. )). ANSYS

Fluent takes the weights from physical models and considers them for partitioning. The weights are

assembled based on the time used by each physical model. For dynamic load balancing, the load is

checked and balanced based on your specified imbalance threshold. To apply dynamic load balancing

on the various models, click the Dynamic Load Balancing tab and select the required balancing as

follows:

Figure . : The Dynamic Load Balancing Tab

. Enable Physical Models load balancing during iterations so that the load will be evaluated for time usage

and weight distribution, based on the Interval that you provide. If the imbalance exceeds the specified

Threshold, then repartitioning will be performed by considering the selected weights. Physical Models

load balancing will only be available when you have the specific physical models enabled in the case.

You will be prompted to enable the weights for those models.When weights for the physical models

are all disabled, you will be prompted to disable Physical Models load balancing.

Note

Applying load balancing too frequently may cause performance degradation due to

the additional cost of migrating cells for the new partition layout.

. Enable Dynamic Mesh if there is any dynamic mesh movement. Load balancing, based on the number

of cells, will be checked and balanced if the imbalance threshold is exceeded.These parallel partitioning

options are provided because with mesh motion, when local remeshing and smoothing are performed,

the partition interface can become very wrinkled and load balance may deteriorate. By default, the Auto

option is selected, where a percentage of interface faces and loads are automatically traced.When this

option is selected, ANSYS Fluent automatically determines the most appropriate repartitioning interval

based on various simulation parameters. However, sometimes, the frequency of load balancing from the

Auto option may be inadequate, and then the Interval setting can be explicitly set.The Interval setting

lets you specify the interval (in time steps or iterations, respectively) when load balancing is enforced.

When load balancing is not desired, you may disable Dynamic Mesh load balancing. Dynamic Mesh

load balancing is only available when you have dynamic models enabled in your case.

Important

Note that when dynamic meshes and local remeshing are utilized, updated meshes

may be slightly different in parallel ANSYS Fluent (when compared to serial ANSYS

Fluent or when compared to a parallel solution created with a different number of

compute nodes), resulting in very small differences in the solutions.

. Enable Mesh Adaption. Any time mesh adaption occurs, load balancing, based on the number of cells,

will be checked and balanced if the imbalance threshold is exceeded. If problems arise in your computa-

tions due to adaption, you can disable the load balancing for Mesh Adaption.

Partitioning the mesh for parallel processing has three major goals:

Create partitions with equal numbers of cells.

Minimize the number of partition interfaces — that is, decrease partition boundary surface area.

Minimize the number of partition neighbors.

Balancing the partitions (equalizing the number of cells) ensures that each processor has an equal load

and that the partitions will be ready to communicate at about the same time. Since communication

between partitions can be a relatively time-consuming process, minimizing the number of interfaces

can reduce the time associated with this data interchange. Minimizing the number of partition

neighbors reduces the chances for network and routing contentions. In addition, minimizing partition

neighbors is important on machines where the cost of initiating message passing is expensive compared

to the cost of sending longer messages. This is especially true for workstations connected in a network.

The partitioning schemes in ANSYS Fluent use bisection or METIS algorithms to create the partitions,

but unlike other schemes that require the number of partitions to be a factor of two, these schemes

have no limitations on the number of partitions. You will create as many partitions as there are com-

puting units (cores based on processors and machines) available for your simulation.

.... Partition Methods

The mesh is partitioned using a bisection or METIS algorithm. The selected algorithm is applied to

the parent domain, and then recursively applied to the subdomains. For example, to divide the mesh

into four partitions with a bisection method, Fluent will bisect the entire (parent) domain into two

child domains, and then repeat the bisection for each of the child domains, yielding four partitions

in total. To divide the mesh into three partitions with a bisection method, Fluent will “bisect” the

parent domain to create two partitions—one approximately twice as large as the other—and then

bisect the larger child domain again to create three partitions in total. METIS uses graph partitioning

techniques that generally provide more optimal partitions than the geometric methods.

The mesh can be partitioned using one of the algorithms listed below. The most efficient choice is

problem-dependent, so you can try different methods until you find the one that is best for your

problem. See Guidelines for Partitioning the Mesh (p. ) for recommended partitioning strategies.

Cartesian Axes

bisects the domain based on the Cartesian coordinates of the cells (see Figure . : Partitions Created

with the Cartesian Axes Method (p. )). It bisects the parent domain and all subsequent child subdomains

perpendicular to the coordinate direction with the longest extent of the active domain. It is often referred

to as coordinate bisection.

Cartesian Strip

uses coordinate bisection but restricts all bisections to the Cartesian direction of longest extent of the

parent domain (see Figure . : Partitions Created with the Cartesian Strip or Cartesian X-Coordinate

Method (p. )).You can often minimize the number of partition neighbors using this approach.

Cartesian X-,Y-, Z-Coordinate

bisects the domain based on the selected Cartesian coordinate. It bisects the parent domain and all

subsequent child subdomains perpendicular to the specified coordinate direction. (See Figure . : Par-

titions Created with the Cartesian Strip or Cartesian X-Coordinate Method (p. ).)

Cartesian R Axes

bisects the domain based on the shortest radial distance from the cell centers to that Cartesian axis ( ,

, or ) whichever produces the smallest interface size.This method is available only in 3D.

Cartesian RX-, RY-, RZ-Coordinate

bisects the domain based on the shortest radial distance from the cell centers to the selected Cartesian

axis ( ,

, or ).These methods are available only in 3D.

Cylindrical Axes

bisects the domain based on the cylindrical coordinates of the cells.This method is available only in 3D.

Cylindrical R-,Theta-, Z-Coordinate

bisects the domain based on the selected cylindrical coordinate.These methods are available only in

3D.

Metis

uses the METIS software package for partitioning irregular graphs, developed by Karypis and Kumar

at the University of Minnesota and the Army HPC Research Center. It uses a multilevel approach

in which the vertices and edges on the fine graph are coalesced to form a coarse graph. The

coarse graph is partitioned, and then uncoarsened back to the original graph. During coarsening

and uncoarsening, algorithms are applied to permit high-quality partitions. METIS routines can

handle partitioning with model-weighted multiple constraints: when automatically partitioning,

solid cell zones are weighted with a default value of . relative to the fluid cell weighting; when

manually partitioning, you can control weighting for cells, solid cell zones, VOF, DPM, and ISAT

table lookup (as described in Partitioning (p. )). Detailed information about METIS can be found

in [] (p. ) and [] (p. ).

Important

If you create non-conformal interfaces, and generate virtual polygonal faces, your

Important

METIS partition can cross non-conformal interfaces by using the connectivity of the

virtual polygonal faces. This improves load balancing for the parallel solver and minim-

izes communication by decreasing the number of partition interface cells.

Polar Axes

bisects the domain based on the polar coordinates of the cells (see Figure . : Partitions Created with

the Polar Axes or Polar Theta-Coordinate Method (p. )).This method is available only in 2D.

Polar R-Coordinate, Polar Theta-Coordinate

bisects the domain based on the selected polar coordinate (see Figure . : Partitions Created with the

Polar Axes or Polar Theta-Coordinate Method (p. )).These methods are available only in 2D.

Principal Axes

bisects the domain based on a coordinate frame aligned with the principal axes of the domain (see

Figure . : Partitions Created with the Principal Axes Method (p. )).This reduces to Cartesian bisection

when the principal axes are aligned with the Cartesian axes.The algorithm is also referred to as moment,

inertial, or moment-of-inertia partitioning.

This is the default bisection method in ANSYS Fluent.

Principal Strip

uses moment bisection but restricts all bisections to the principal axis of longest extent of the parent

domain (see Figure . : Partitions Created with the Principal Strip or Principal X-Coordinate Meth-

od (p. )).You can often minimize the number of partition neighbors using this approach.

Principal X-,Y-, Z-Coordinate

bisects the domain based on the selected principal coordinate (see Figure . : Partitions Created with

the Principal Strip or Principal X-Coordinate Method (p. )).

Spherical Axes

bisects the domain based on the spherical coordinates of the cells.This method is available only in 3D.

Spherical Rho-,Theta-, Phi-Coordinate

bisects the domain based on the selected spherical coordinate.These methods are available only in 3D.

Figure . : Partitions Created with the Cartesian Axes Method

Figure . : Partitions Created with the Cartesian Strip or Cartesian X-Coordinate Method

Figure . : Partitions Created with the Principal Axes Method

Figure . : Partitions Created with the Principal Strip or Principal X-Coordinate Method

Figure . : Partitions Created with the Polar Axes or Polar Theta-Coordinate Method

.... Optimizations

Additional optimizations can be applied to improve the quality of the mesh partitions. The heuristic

of bisecting perpendicular to the direction of longest domain extent is not always the best choice

for creating the smallest interface boundary. A pre-testing operation (for details, see Pretesting (p. ))

can be applied to automatically choose the best direction before partitioning. In addition, the following

iterative optimization schemes exist:

Smooth

attempts to minimize the number of partition interfaces by swapping cells between partitions.The

scheme traverses the partition boundary and gives cells to the neighboring partition if the interface

boundary surface area is decreased. (See Figure . :The Smooth Optimization Scheme (p. ).)

Merge

attempts to eliminate orphan clusters from each partition. An orphan cluster is a group of cells with the

Merge

common feature that each cell within the group has at least one face that coincides with an interface

boundary. (See Figure . :The Merge Optimization Scheme (p. ).) Orphan clusters can degrade

multigrid performance and lead to large communication costs.

Figure . : The Smooth Optimization Scheme

Figure . : The Merge Optimization Scheme

In general, the Smooth and Merge schemes are relatively inexpensive optimization tools.

.... Pretesting

If you choose the Principal Axes or Cartesian Axes method, you can improve the bisection by testing

different directions before performing the actual bisection. If you choose not to use pretesting (the

default), ANSYS Fluent will perform the bisection perpendicular to the direction of longest domain

extent.

If pretesting is enabled, it will occur automatically when you click the Partition button in the Parti-

tioning and Load Balancing Dialog Box (p. ), or when you read in the mesh if you are using auto-

matic partitioning. The bisection algorithm will test all coordinate directions and choose the one

which yields the fewest partition interfaces for the final bisection.

Note that using pretesting will increase the time required for partitioning. For 2D problems partitioning

will take  times longer than without pretesting, and for 3D problems it will take  times longer.

.... Using the Partition Filter

As noted above, you can use the METIS partitioning method through a filter in addition to within the

Auto Partition Mesh and Partitioning and Load Balancing dialog boxes. To perform METIS parti-

tioning on an unpartitioned mesh, use the File/Import/Partition/Metis... ribbon tab item.

ANSYS Fluent will use the METIS partitioner to partition the mesh, and then read the partitioned

mesh. The number of partitions will be equal to the number of processes. You can then proceed with

the model definition and solution.

Important

Direct import to the parallel solver through the partition filter requires that the host machine

has enough memory to run the filter for the specified mesh. If not, you must run the filter

on a machine that does have enough memory. You can either start the parallel solver on

the machine with enough memory and repeat the process described above, or run the

filter manually on the new machine and then read the partitioned mesh into the parallel

solver on the host machine.

To manually partition a mesh using the partition filter, enter the following command:

utility partition input_filename partition_count output_filename

where input_filename is the filename for the mesh to be partitioned, partition_count is the number

of partitions desired, and output_filename is the filename for the partitioned mesh. You can then read

the partitioned mesh into Fluent (using the standard File/Read/Case... ribbon tab item) and proceed

with the model definition and solution.

When the File/Import/Partition/Metis... ribbon tab item is used to import an unpartitioned mesh

into the parallel solver, the METIS partitioner partitions the entire mesh. You may also partition each

cell zone individually, using the File/Import/Partition/Metis Zone... ribbon tab item.

This method can be useful for balancing the work load for cases that have few cell zones.

After partitioning a mesh, you should check the partition information and examine the partitions

graphically.

.... Interpreting Partition Statistics

You can request a report to be displayed after partitioning (either automatic or manual) is completed.

Click the Print Active Partitions or Print Stored Partitions button in the Partitioning and Load

Balancing dialog box.

ANSYS Fluent distinguishes between two cell partition schemes: the active cell partitions and the

stored cell partitions. Initially, both are set to the cell partitions that were established upon reading

the case file. If you re-partition the mesh using the Partitioning and Load Balancing dialog box, the

new partitions will be referred to as the stored cell partitions. To make them the active cell partitions,

you must click the Use Stored Partitions button in the Partitioning and Load Balancing dialog box

in the parallel version of ANSYS Fluent. The active cell partitions are used for the current calculation,

while the stored cell partitions (determined from the last partitioning performed) are used when you

save a case file. This distinction is made mainly to allow you to partition a case on one machine or

network of machines and solve it on a different one. Thanks to the two separate partitioning schemes,

you could use the parallel solver with a certain number of compute nodes to subdivide a mesh into

an arbitrary different number of partitions, suitable for a different parallel machine, save the case file,

and then load it into the designated machine.

The output generated when you print the partitions consists of tabulated information about the

active or stored partitioning scheme. A typical output for a mesh with  partitions is as follows:

P   Cells I-Cells Cell Ratio   Faces I-Faces Face Ratio Neighbors Load

. .

. .

. .

. .

Collective Partition Statistics:        Minimum   Maximum   Total

Cell count

Mean cell count deviation               -.%     .%

Partition boundary cell count ratio     .%      .%      .%

Face count

Mean face count deviation               -.%     .%

Partition boundary face count ratio     .%      .%      .%

Partition Method                        Metis

The first table in the output displays per-partition statistics of interest:

P

the partition ID

Cells

the number of cells in the partition

I-Cells

the number of interface cells in the partition (that is, cells that lie on the partition interfaces)

Cell Ratio

the ratio of interface cells to total cells for the partition

Faces

the number of faces in the partition

I-Faces

the number of interface faces in the partition (that is, faces that lie on partition interfaces)

Face Ratio

Faces

I-Faces

Face Ratio

the ratio of interface faces to total faces for the partition

Neighbors

the number of neighbor partitions

Load

the desired relative load on this node in proportion to the other nodes. See Load Distribution (p. )

Note that partition IDs correspond directly to compute node IDs when a case file is read into the

parallel solver. When the number of partitions in a case file is larger than the number of compute

nodes, but is evenly divisible by the number of compute nodes, then the distribution is such that

partitions with IDs  to

are mapped onto compute node , partitions with IDs

to

onto compute node , and so on, where

is equal to the ratio of the number of partitions to the

number of compute nodes.

The second table in the output displays Minimum, Maximum, and (where applicable) Total values

for various partition statistics:

Cell Count

the number of cells in the partitions (corresponding to Cells in the per-partition table)

Mean cell count deviation

the deviation of an individual partition cell count from the mean partition cell count

the number of cells that lie on partition interfaces (corresponding to I-Cells in the per-partition

table)

Partition boundary cell count ratio

the ratio of the number of cells that lie on partition interfaces to the total number of cells in the

partition (corresponding to Cell Ratio in the per-partition table)

Face Count

the number of faces in the partitions (corresponding to Faces in the per-partition table)

Mean face count deviation

Face Count

the deviation of an individual partition face count from the mean partition face count

the number of faces that lie on partition interfaces (corresponding to I-Faces in the per-partition

table)

Partition boundary face count ratio

the ratio of the number of faces that lie on partition interfaces to the total number of faces in the

partition (corresponding to Face Ratio in the per-partition table)

the number of neighbors for a given partition (corresponding to Neighbors in the per-partition

table)

Finally, the Partition Method and Stored Partition Count are displayed.

Your aim is to minimize the Maximum value of the Partition boundary face count ratio,

while maintaining a balanced load. For a given mesh, the Mean cell count deviation is a

measure of the maximum load imbalance for a method. If the statistics are not satisfactory for a

problem, you can try one of the other partitioning methods.

If there is an overset mesh for which the solution has been initialized, an additional partition table

with solve and dead cells is included in the partitioning report (see Overset Cell Marks (p. ) for the

definitions of such cells):

>> Overset partition statistics:

P   Cells Solve-cells Dead-cells  Ext donors

Overset Partition Statistics:           Minimum   Maximum   Total

Cell count

Cell count

Mean cell count deviation               .%      .%

Solve cell count

Mean solve cell count deviation         -.%     .%

Dead cell count

Mean dead cell count deviation          .%      .%

Ext donors

.... Examining Partitions Graphically

To further aid interpretation of the partition information, you can draw contours of the mesh partitions

(see the figures in Partition Methods (p. )).

Edit...

To display the active cell partition or the stored cell partition (which were described above), select

Active Cell Partition or Stored Cell Partition in the Cell Info... category of the Contours Of drop-

down list, and turn off the display of Node Values (for details, see Displaying Contours and Pro-

files (p. ) for information about displaying contours).

Important

If you have not already done so in the setup of your problem, you must perform a solution

initialization in order to use the Contours dialog box.

If the speeds of the processors that will be used for a parallel calculation differ significantly, you can

specify a load distribution for partitioning, using the load-distribution text command.

parallel → partition → set → load-distribution

For example, if you will be solving on three compute nodes, and one machine is twice as fast as the

other two, then you may want to assign twice as many cells to the first machine as to the others (that

is, a load vector of (  )). During subsequent mesh partitioning, partition  will end up with twice

as many cells as partitions  and .

For this example, you need to start up ANSYS Fluent such that compute node  is the fast machine,

since partition , with twice as many cells as the others, will be mapped onto compute node . Altern-

atively, in this situation, you could enable the load balancing feature (described in Load Balan-

cing (p. )) to have ANSYS Fluent automatically attempt to discern any difference in load among the

compute nodes.

When running a calculation using parallel ANSYS Fluent, you may encounter a warning message in

the console that reports problems related to the partitioning. The following is an example of such a

warning:

#AMG# Warning: The global matrix size () is too large, and may

adversely affect the parallel performance. See the ANSYS Fluent User's

Guide for information on troubleshooting partitioning issues.

The following are possible reasons for partitioning problems, along with recommendations for reducing

them:

The presence of solid zones may cause a partition to have a very small amount of fluid cells, or none

at all. To avoid this, it is recommended that you use the Metis method with automatic or manual

partitioning; for the latter, you must ensure that Solid Zones weighting and model-weighted parti-

tioning are enabled, with a suitable Value for the solid-to-fluid cell weighting (for example, . ).

A partition may have a small number of cells if you have set up a load distribution for partitioning. Such

settings should be disabled, by using the load-distribution text command (described in Load Distri-

bution (p. )) and entering a value of  for each of the previously defined partitions.

Some model settings (for example, shell conduction) can encapsulate some cells, which may cause difficulties

with the coarsening process.To remedy this situation, you can either try a different partitioning method,

or you can enable the global coarsening checking criteria with the following rpvar setting:

(rpsetvar 'amg/parallel/global-check-coarsening? #t)

Coupled walls are encapsulated as part of the shell conduction model and S2S model. If you have

partitioning problems, you can try reverting to the encapsulation routine used prior to version .

by disabling the enhanced encapsulation:

define → models → shell-conduction → enhanced-encapsulation?

.. Using General Purpose Graphics Processing Units (GPGPUs) With

the Algebraic Multigrid (AMG) Solver

You can accelerate the Algebraic Multigrid (AMG) solver inside Fluent using General Purpose Graphics

Processing Units (GPGPUs) if suitable hardware is available on your compute machines. When enabled,

you can use GPGPU acceleration for AMG computations in a Fluent session on linear systems with up

to  coupled equations. Using GPGPUs requires HPC licenses. Licensing details can be found in HPC Li-

censing in the ANSYS, Inc. Licensing Guide.

Using General Purpose Graphics Processing Units (GPGPUs) With the Algebraic

Multigrid (AMG) Solver

... Requirements

GPUs that are supported in the current release are posted on the Platform Support section of the

ANSYS Website.

When starting the parallel Fluent session the following conditions must be met:

The number of solver processes per machine must be equal on all machines.

The number solver processes per machine must be evenly divisible by the specified number of GPGPUs

per machine.

GPGPU acceleration is subject to the following limitations:

When using Fluent in Workbench, the number of GPGPUs cannot be set through:

– Properties of Setup Cells

– Properties of Solution Cells

– Properties of Solution Cells through RSM update

– Properties of Parameter Sets through RSM update

GPGPU acceleration will not be used in the following cases:

– The population balance model is active.

– The Eulerian multiphase model is active.

– The system has more than  coupled equations.

... Using and Managing GPGPUs

In order to use GPGPUs, you must specify in the Fluent Launcher or with the -gpgpu= ngpgpus

command line option how many GPGPUs are to be used per machine (note that when launching in

serial, the command line option is the only available way to specify the GPGPUs). For details, refer to

the following sections:

Starting Parallel ANSYS Fluent Using Fluent Launcher (p. )

Starting Parallel ANSYS Fluent on a Windows System Using Command Line Options (p. )

Starting Parallel ANSYS Fluent on a Linux System (p. )

Once the Fluent session is running, you can view and/or select the available GPGPUs on the system

using the following TUI commands:

parallel/gpgpu/show

display the available GPGPUs on the system.

parallel/gpgpu/select

select the GPGPUs to use. Note that you can only select up to the number of GPGPUs that you specified

on the command line or in the Fluent Launcher when starting the session.

By default, GPGPU acceleration is applied automatically to coupled systems and not to scalar systems

because scalar systems typically are not as computationally expensive. However, if desired you can

enable/disable GPGPU acceleration of the AMG solver for coupled and scalar systems in the following

TUI menu:

solve/set/amg-options/amg-gpgpu-options/

The menu contains commands for each supported equation type allowing you to enable/disable GPGPU

acceleration, choose between AMG and FGMRES solvers, and specify various solver options.

You can control the maximum number of threads on each machine by using the Thread Control dialog

box (Figure . : The Parallel Connectivity Dialog Box (p. )).

Parallel → General → Thread Control...

machine is equal to the number of ANSYS Fluent node processes on each machine.

number of cores on the machine. ANSYS Fluent obtains the number of cores from the OS. This may

be applicable when the multi-threaded part of the calculation is dominating the computation time,

and the continuous phase calculation is relatively small, and you want to take full advantage of the

computation resources. For example, if you have a very small case with regard to the number of cells,

but a large number of particles to be tracked, you may want to spawn one ANSYS Fluent node process

on each machine, but use the maximum number of cores in order to get a good overall performance.

Controlling the Threads

you want to have fine control of the number of threads on each machine; it is not recommended in

general.

For any compute node, you can print network connectivity information that includes the hostname,

architecture, process ID, and ID of the selected compute node and all machines connected to it. The

ID of the selected compute node is marked with an asterisk.

The ID for the ANSYS Fluent host process is always host. The compute nodes are numbered sequentially

starting from node-. All compute nodes are completely connected. In addition, compute node  is

connected to the host process.

To obtain connectivity information for a compute node, you can use the Parallel Connectivity Dialog

Box (p. ) (Figure . : The Parallel Connectivity Dialog Box (p. )).

Parallel → Network → Connectivity...

Figure . : The Parallel Connectivity Dialog Box

Indicate the compute node ID for which connectivity information is desired in the Compute Node field,

and then click the Print button. Sample output for compute node  is shown below:

-----------------------------------------------------------------------------------------------

ID      Hostname              Core        O.S. PID     Vendor

n5      host25                /        Linux-       AMD Opteron(tm)

n2      host25                /        Linux-       AMD Opteron(tm)

n4      host24                /        Linux-       AMD Opteron(tm)

n1      host24                /        Linux-       AMD Opteron(tm)

host    host23                -           Linux-       AMD Opteron(tm)

n3      host23                /        Linux-       AMD Opteron(tm)

n0*     host23                /        Linux-       AMD Opteron(tm)

Fluent offers several tools to help you optimize the performance of your parallel computations. You

can check the utilization of your hardware using the parallel check feature. To determine how well the

parallel solver is working, you can measure computation and communication times, and the overall

parallel efficiency, using the performance meter. You can also control the amount of communication

between compute nodes in order to optimize the parallel solver, and take advantage of the automatic

load balancing feature of ANSYS Fluent.

Information about checking and improving parallel performance is provided in the following sections:

... Parallel Check

... Checking Parallel Performance

... Optimizing the Parallel Solver

... Clearing the Linux File Cache Buffers

You can use the Check command in the Parallel ribbon tab to check various factors that affect parallel

performance. Checks are performed to identify the following issues:

CPU cores are overloaded

CPU clock is throttled

System memory usage is too high

A faster interconnect is available

Partitions are imbalanced (if a valid mesh is loaded)

The performance meter allows you to report the wall clock time elapsed during a computation, as well

as message-passing statistics. Since the performance meter is always enabled, you can access the

statistics by displaying them after the computation is completed. To view the current statistics, click

Usage in the Parallel ribbon tab (Timer group box).

Parallel → Timer → Usage

Performance statistics will be displayed in the console.

To clear the performance meter so that you can eliminate past statistics from the future report, click

Reset in the Parallel ribbon tab (Timer group box).

Parallel → Timer → Reset

The following example demonstrates how the current parallel statistics are displayed in the console:

Average wall-clock time per iteration:            . sec

Global reductions per iteration:                     ops

Global reductions time per iteration:             . sec (.%)

Message count per iteration:                         messages

Data transfer per iteration:                      . MB

LE solves per iteration:                             solves

LE wall-clock time per iteration:                 . sec (.%)

LE global solves per iteration:                       solves

LE global wall-clock time per iteration:          . sec (.%)

AMG cycles per iteration:                             cycles

Relaxation sweeps per iteration:                    sweeps

Relaxation exchanges per iteration:                  exchanges

Total wall-clock time:                            . sec

A description of the parallel statistics is as follows:

Checking and Improving Parallel Performance

Average wall-clock time per iteration describes the average real (wall clock) time per iter-

ation.

Global reductions per iteration describes the number of global reduction operations (such

as variable summations over all processes).This requires communication among all processes.

A global reduction is a collective operation over all processes for the given job that reduces a vector

quantity (the length given by the number of processes or nodes) to a scalar quantity (for example,

taking the sum or maximum of a particular quantity). The number of global reductions cannot be

calculated from any other readily known quantities. The number is generally dependent on the al-

gorithm being used and the problem being solved.

Global reductions time per iteration describes the time per iteration for the global reduction

Message count per iteration describes the number of messages sent between all processes per

iteration.This is important with regard to communication latency, especially on high-latency interconnects.

A message is defined as a single point-to-point, send-and-receive operation between any two pro-

cesses. This excludes global, collective operations such as global reductions. In terms of domain

decomposition, a message is passed from the process governing one subdomain to a process gov-

erning another (usually adjacent) subdomain.

The message count per iteration is usually dependent on the algorithm being used and the problem

being solved. The message count and the number of messages that are reported are totals for all

processors.

The message count provides some insight into the impact of communication latency on parallel

performance. A higher message count indicates that the parallel performance may be more adversely

affected if a high-latency interconnect is being used. Ethernet has a higher latency than Infiniband.

Therefore, a high message count will more adversely affect performance with Ethernet than with

Infiniband.

To check the latency of the overall cluster interconnect, refer to Checking Latency and Band-

width (p. ).

Data transfer per iteration describes the amount of data communicated between processors

per iteration.This is important with respect to interconnect bandwidth.

Data transfer per iteration is usually dependent on the algorithm being used and the problem being

solved. This number generally increases with increases in problem size, number of partitions, and

physics complexity.

The data transfer per iteration may provide some insight into the impact of communication bandwidth

(speed) on parallel performance. The precise impact is often difficult to quantify because it is de-

pendent on many things including: ratio of data transfer to calculations, and ratio of communication

bandwidth to CPU speed. The unit of data transfer is a byte.

To check the bandwidth of the overall cluster interconnect, refer to Checking Latency and Band-

LE solves per iteration describes the number of linear systems being solved per iteration.This

number is dependent on the physics (non-reacting versus reacting flow) and the algorithms (pressure-

based versus density-based solver), but is independent of mesh size. For the pressure-based solver, this is

usually the number of transport equations being solved (mass, momentum, energy, and so on).

LE wall-clock time per iteration describes the time (wall-clock) spent doing linear equation

solvers (that is, multigrid).

LE global solves per iteration describes the number of solutions on the coarsest level of the

AMG solver where the entire linear system has been pushed to a single processor (n0).The system is pushed

to a single processor to reduce the computation time during the solution on that level. Scaling generally

is not adversely affected because the number of unknowns is small on the coarser levels.

LE global wall-clock time per iteration describes the time (wall-clock) per iteration for

the linear equation global solutions.

AMG cycles per iteration describes the average number of multigrid cycles (V,W, flexible, and

so on) per iteration.

Relaxation sweeps per iteration describes the number of relaxation sweeps (or iterative solu-

tions) on all levels for all equations per iteration. A relaxation sweep is usually one iteration of Gauss-Siedel

or ILU.

Relaxation exchanges per iteration describes the number of solution communications between

processors during the relaxation process in AMG.This number may be less than the number of sweeps

because of shifting the linear system on coarser levels to a single node/process.

Time-step updates per iteration describes the number of sub-iterations on the time step per

iteration.

Time-step wall-clock time per iteration describes the time per sub-iteration.

Total wall-clock time describes the total wall-clock time.

The most relevant quantity is the Total wall clock time. This quantity can be used to gauge

the parallel performance (speedup and efficiency) by comparing this quantity to that from the serial

analysis.

.... Checking Latency and Bandwidth

You can check the latency and bandwidth of the overall cluster interconnect, to help identify any issues

affecting ANSYS Fluent scalability, by clicking Latency and Bandwidth in the Parallel ribbon tab

(Network group box).

Parallel → Network → Latency

Depending on the number of machines and processors being used, a table containing information

about the communication speed for each node will be displayed in the console. The table will also

summarize the minimum and maximum latency between two nodes.

Consider the following example when checking for latency:

Latency (usec) with  samples [. sec]

------------------------------------------

ID       n0     n1     n2    n3    n4    n5

n0            . . . . *

n1    . . . . *

n0            . . . . *

n1    . . . . *

n2    . . . . *

n3    . . *        . .

n4    . . . . *

n5    . . *  . .

Min: . [n0<-->n1]

Max: . [n5<-->n2]

Important

In the above table, (*) is the maximum value in that row. The smaller the latency, the better.

Six processors (n0 to n5) are spawned. The latency between n0 and n1 is .

. Similarly, the latency

between n1 and n2 is .

. The minimum latency occurs between n0 and n1 and the maximum

latency occurs between n2 and n5, as noted in the table. Checking the latency is particularly useful

when you are not seeing expected speedup on a cluster.

Parallel → Network → Bandwidth

In addition to checking for latency, you can check your bandwidth. A table containing information

about the amount of data communicated within one second between two nodes is displayed in the

console. The table will also summarize the minimum and maximum bandwidth between two nodes.

Consider the following example when checking for bandwidth:

Bandwidth (MB/s) with  messages of size 4MB [. sec]

--------------------------------------------

ID      n0     n1     n2     n3     n4     n5

n0          . *  . . .

n1   . . . . *

n2    . . . . *

n3   . . . . *

n4    . . . *          .

n5   . . . *    .

Min: . [n5<-->n3]

Max: . [n0<-->n3]

Important

In the above table, (*) is the minimum value in that row. The larger the bandwidth, the

Important

better.

The bandwidth between n0 and n1 is . MB/s. Similarly, the bandwidth between n1 and n2 is .

MB/s. The minimum amount of bandwidth occurs between n3 and n5 and the maximum occurs

between n0 and n3, as noted in the table. Checking the bandwidth is particularly useful when you

cannot see good scalability with relatively large cases.

.... Increasing the Report Interval

In ANSYS Fluent, you can reduce communication and improve parallel performance by increasing the

report interval for residual printing/plotting or other solution monitoring reports. You can modify the

value for Reporting Interval in the Run Calculation Task Page (p. ).

Calculate...

Important

Note that you will be unable to interrupt iterations until the end of each report interval.

.... Accelerating View Factor Calculations for General Purpose Computing on

Graphics Processing Units (GPGPUs)

View factor computations can be accelerated through the viewfac_acc utility that uses a combin-

ation of MPI/OpenMP/OpenCL models to speed up view factor computations. Irrespective of the

number of MPI processes launched, only one MPI process/machine is used for computing view factors.

On each machine, one MPI process spawns several OpenMP threads that actually compute the view

factors. Since only one MPI process is required per machine, it is recommended that you start just

one MPI process per machine and specify the number of OpenMP threads to use when running the

utility outside of ANSYS Fluent. With fewer MPI processes, the system memory usage is reduced as

well. When running the utility from inside ANSYS Fluent, the number of viewfac_acc processes

will be same as the number of ANSYS Fluent processes. If OpenCL-capable GPUs are available, then

a portion of the view factor computations are done on GPUs using OpenCL, to further speed up the

computation. At present, this capability is limited to the hemicube method with the cluster-to-cluster

option on lnamd64 and win64 machines.

When using the utility viewfac_acc outside of ANSYS Fluent, you can specify the following command

line options:

-cpu # (default = -) The number of OpenMP threads to launch per machine.

– -:The number of MPI processes.

– -:The total number of logical CPU cores.

– : No CPU used.

– n: Up to maximum n.

-gpu # (default = ) The number of GPU devices to use per machine.

– –:The total number of GPU devices.

– : No GPU used.

-gpu_cpu_ratio # (default = .) The ratio of the work load on  GPU vs  CPU OpenMP thread.

This is based on the time consumed by the GPU and the CPU. At the end of the view factor computa-

tions, a recommendation is printed for the GPU/CPU work load ratio to use in future computations.

When using the viewfac_acc utility from inside an ANSYS Fluent session, use the

/define/models/radiation/s2s-parameters/compute-clusters-and-vf-acceler-

ated text interface (TUI) command. You will only be prompted for the -gpu and -gpu_cpu_ratio

options (as described previously) and not the -cpu option, as the number of OpenMP threads to

launch per machine can be specified in the Thread Control Dialog Box (p. ) (see Controlling the

Threads (p. ) for details).

In order to use the GPU for view factor computations, the OpenCL library should be accessible through

the appropriate environment variable (LD_LIBRARY_PATH on lnamd64 or %path% on win64). By

default on lnamd64, /usr/lib64 is searched, but if the library is installed in another location, then

that location should be specified in the LD_LIBRARY_PATH variable.

View factor computations can also be accelerated through the raytracing_acc utility that uses

the NVIDIA Optix library for tracing the rays. The GPU available on the machine running the host

process is used in such a scenario, except in a mixed Windows-Linux simulation where the GPU on

node- is used. An NVIDIA GPU along with CUDA . is required for using raytracing_acc. At

present, this utility is available only on lnamd64 (Red Hat Enterprise Linux /, and SUSE Linux Enter-

prise Server ) and win64 (Windows ) machines for 3D problems. In order to use the utility, the

CUDA . library should be accessible through the appropriate environment variable (LD_LIB-

RARY_PATH on lnamd64 or %path% on win64).

When using the raytracing_acc utility from outside an ANSYS Fluent session, the command line

is utility raytracing_acc <input_cluster_file> [output_s2s_file(optional)].

When using the raytracing_acc utility from inside an ANSYS Fluent session, use the

ated text user interface (TUI) command.

.... Accelerating Discrete Ordinates (DO) Radiation Calculations

The accelerated discrete ordinates (DO) radiation solver is computationally faster than the standard

DO solver. Note that even though the accelerated DO solver may take more iterations to converge,

the overall simulation time is shorter.

After you have selected the DO model in the Radiation Model dialog box, you can enable the accel-

erated DO solver by using the following text command:

define → models → radiation → do-acceleration?

If NVIDIA GPGPUs are enabled in the Fluent session, this solver will accelerate the DO computations

by using the GPGPUs. In the absence of GPGPUs, this solver can still be used with the CPU cores to

accelerate the DO computations. Note that the accelerated DO solver uses the first-order upwind

scheme (and ignores whatever selection you have made for the Discrete Ordinates spatial discretiz-

ation scheme in the Solution Methods task page), along with an explicit relaxation of ..

The accelerated DO solver is incompatible with some models and settings; when necessary, Fluent

will automatically revert to the standard DO solver when the calculation is started and print a message

about the conflict.

If you plan to use GPGPUs with the accelerated DO solver, it is recommended that you run NVIDIA’s

multi-process server (MPS) before launching ANSYS Fluent using the following command: nvidia-

cuda-mps-control -d. It is known to improve the robustness and performance of the GPGPU

computations with the multiple Fluent processes.

Processing performance can significantly decrease when the file cache buffers of a Linux machine are

full. While this is true in serial, it is more often a concern when solving large cases in parallel, particularly

when using AMD processors. If you see a performance decrease even though the case / machine setup

has not changed, that is an indication that the file cache buffers may be to blame.

The filling of the file cache buffers can happen over a period of time as a result of input-output activity.

Even after the ANSYS Fluent session is exited, by default the operating system does not free up the

file cache buffers immediately (unless the operating system is unable to satisfy a malloc subroutine

request with available free memory). During memory allocation for a parallel case, this can result in

the allocation of memory from a different NUMA domain, and consequently can have a significant

impact on performance.

To resolve this issue on Linux machines, you must first ensure that all of the relevant machines are

idle (so that you do not adversely affect any jobs that are running). Then you can clear the file cache

buffers by performing one of the following actions:

Include the -cflush option when launching ANSYS Fluent from the command line.

This option ensures that the file cache buffers are flushed in a separate operation. While this process

may take a few minutes to complete (depending on the total memory of the system), it does not

require you to have root privileges.

or

Enter the (drop-cache) Scheme command (either in the ANSYS Fluent console or through your journal

or

file) after launching Fluent but before you read the case file.

This command will instantaneously clear the pagecaches, dentries, and inodes.

Important

Note that in order to use the (drop-cache) command, you must have sudo adminis-

trative privileges for the /sbin/sysctl vm.drop_caches= command.

Chapter : Design Analysis and Optimization

In this chapter, the setup and use of the adjoint solver and the mesh morpher/optimizer in ANSYS Fluent

are described. Both tools offer shape optimization capabilities, but the scope is complementary. The

fundamental difference in the technology is that the adjoint solver uses gradient-based optimization

by calculating derivatives, whereas the mesh morpher/optimizer uses a strategy that is not based on

gradients to decide design updates.

The tools have a common approach to change a design by morphing the computational mesh. This

has the benefit that you need not return to the original geometry in order to update the design for the

purposes of the optimization.

The two key considerations when deciding whether to use the adjoint solver or the mesh morpher/op-

timizer are as follows:

Is the flow physics / observable of interest supported by the adjoint solver? (For details about adjoint cap-

abilities, see the following sections: Basic Assumptions and Consistency Checks (p. ) and General Observ-

ables (p. )) If not, then the mesh morpher/optimizer is the better option, since there are very few limitations

in the supported physics and choice of quantity of interest with this approach. It is important to verify that

the quantity of interest can be specified as an adjoint solver observable.

Is the dimension of the design space high? Detailed shape optimization of 3D geometries can involve design

spaces with large dimensions (thousands of degrees of freedom or more).The adjoint solver is very effective

in this scenario, whereas the use of the mesh morpher/optimizer becomes computationally prohibitive

when the number of degrees of freedom exceeds more than, say, –.

..The Adjoint Solver

.. Using the Adjoint Solver

..The Mesh Morpher/Optimizer

.. Using the Mesh Morpher/Optimizer

An adjoint solver is a specialized tool that extends the scope of the analysis provided by a conventional

flow solver by providing detailed sensitivity data for the performance of a fluid system.

In order to perform a simulation using the ANSYS Fluent standard flow solvers, a user supplies system

geometry in the form of a computational mesh, specifies material properties and physics models, and

configures boundary conditions of various types. The conventional flow solver, once converged, provides

a detailed data set that describes the flow state governed by the flow physics that are being modeled.

Various postprocessing steps can be taken to assess the performance of the system.

If a change is made to any of the data that defines the problem, then the results of the calculation can

change. The degree to which the solution changes depends on how sensitive the flow is to the partic-

ular parameter that is being adjusted. Indeed, the derivative of the solution data with respect to that

parameter quantifies this sensitivity to first order. Determining these derivatives is the domain of sens-

itivity analysis.

There is a large collection of derivative data that can be computed for a fluid system, given the extensive

set of input data that is required, and the extensive flow data that is produced. The matrix of derivatives

of output data with respect to input data can be vast. Depending upon the goal of the analysis only a

portion of this derivative data may be needed for engineering analysis and decision-making.

The adjoint solver accomplishes the remarkable feat of calculating the derivative of a single engineering

observation with respect to a very large number of input parameters simultaneously via a single compu-

tation. The engineering observation could be a measure of the system performance, such as the lift or

drag on an airfoil, or the total pressure drop through a system. Most importantly, the derivatives with

respect to the geometric shape of the system are found.

Understanding such sensitivities in a fluid system can provide extremely valuable engineering insight.

A system that is highly sensitive may exhibit strong variability in performance due to small variations

in manufacturing or variations in the environment in which it is operating. Alternatively, high-sensitivity

may be leveraged for fluid control, with a small actuator being able to induce strong variations in be-

havior. Yet another perspective is that sensitivity of a performance measure implies that the device in

question is not fully optimized and there is still room for improvement—assuming that constraints do

not preclude further gains.

The sensitivities of a fluid system provided by an adjoint solver satisfy a central need in gradient-based

shape optimization. This makes an adjoint solver a unique and powerful engineering tool for design

optimization.

Adjoint data can also play a role in improving solver numerics. Regions of high sensitivity are indicative

of areas in the flow where discretization errors can potentially have a strong effect. This information

can be used to guide how best to refine a mesh to improve flow solution accuracy.

The process of computing an adjoint solution resembles that for a standard flow calculation in many

respects. The adjoint solver solution advancement method is specified, residual monitors configured,

and the solver is initialized and run through a sequence of iterations to convergence. One notable dif-

ference is that a scalar-valued observation is selected as being of interest prior to starting the adjoint

Once the adjoint solution is converged the derivative of the observable with respect to the position of

each and every point on the surface of the geometry is available, and the sensitivity of the observation

to specific boundary condition settings can be found. This remarkable feature of adjoint solutions has

been known for hundreds of years, but only in the last few decades has the significance for computa-

tional physics analysis been recognized widely.

The power of this methodology is highlighted when an alternative for assembling the same information

is considered. Imagine a sequence of flow calculations in which each point on an airfoil surface is moved

in turn a set small distance in the surface-normal direction, and the flow and drag recomputed. If there

are

points on the surface, then

flow calculations are required to build the data set. Considering

that the same data is provided by a single adjoint computation, the adjoint approach has an enormous

advantage. Remember that for even modest 3D flow computations there may be many thousands of

coordinates or more on a surface.

Once the adjoint is computed it can be used to guide intelligent design modifications to a system. After

all, the adjoint sensitivity data provides a map across the entire surface of the geometry of the effect

of moving the surface. Design modifications can be most effective if made in regions of high sensitivity

since small changes will have a large effect upon the engineering quantity of interest. This principle of

making changes to a system in proportion to the local sensitivity is the foundation for the simple

gradient algorithm for design optimization.

Design Analysis and Optimization

Once a candidate change in shape or other boundary condition has been selected, the effect of that

change can be estimated using the computed derivative data. This amounts to a first order extrapolation

using a Taylor series expansion around the baseline flow state. Clearly if a modification is chosen that

is large enough that nonlinear effects become important then the accuracy of the predicted change

cannot be guaranteed.

... General Observables

Several observables are available and serve as the foundation for specifying the quantity that is of in-

terest for the computation. Basic quantities such as forces and moments can be defined and each is

given a name. The following types of observables are available:

Force: the aerodynamic force in a specified direction on one or more walls.

Moment of force: the aerodynamic moment about a specified moment center and moment axis.The integ-

ration is made over a specified collection of wall zones. Note that in 2D, the moment axis is normal to the

plane of the flow.

Swirl: the moment of the mass flow (with velocity ) relative to an axis defined by a point,

, and a direction

.The two options are:

– Swirl integral

(.)

where

denotes the volume over which the integration is made, and  denotes the relative

position to the point

.

– Normalized swirl integral

(.)

Note

These integrals can be used to construct quantities such as tumble ratio that are of signi-

ficance for internal combustion engine analysis.

pressure drop between an inlet (or group of inlets) and an outlet (or group of outlets)

The total pressure is computed by area-weighted averaging of the total pressure values on selected

surfaces.

fixed value: a simple fixed value can be specified and used in the assembly of the observables.This is con-

venient when some scaling or normalization of the observable is desired. It must be noted that this value

is treated strictly as a constant for the purposes of any derivative calculations.

surface integral: a variety of surface integrals can be constructed for a specified field variable on a

set of user-selected surfaces (including zone surfaces, isosurfaces, and clipped surfaces).

The Adjoint Solver

– Facet sum: a simple sum of the field value on each facet of the computational mesh.

(.)

– Facet average: the facet sum is divided by the total number of facets,

.

(.)

– Facet variance: the sum of the squares of the deviations from the facet average divided by the total

number of facets.

(.)

– Integral: the sum of the field value on each face multiplied by the face area.

(.)

– Area-weighted average: the integral divided by the total face area.

(.)

– Area-weighted variance: the sum of the squares of the deviations from the area-weighted average, divided

by the total face area.

(.)

– Mass-weighted integral: the sum of the field value on each face, weighted by the magnitude of the local

mass flow through the face.

(.)

– Mass-weighted average integral: the mass-weighted integral divided by the sum of the magnitudes of

the local mass flow rates through the faces on which the integral is defined.

(.)

– Mass-weighted variance: the mass-weighted integral of the square of the deviation from the mass-

weighted average, divided by the sum of the magnitudes of the local mass flow rates through the faces

on which the integral is defined.

(.)

– Flow-rate weighted: the rate at which the field is convected through the defined surfaces.

(.)

– The field variables that can be used are:

→ Pressure

→ Total pressure

→ Mass flow per unit area

→ Temperature (when adjoint energy is enabled)

→ Total temperature (when adjoint energy is enabled)

→ Heat flux (when adjoint energy is enabled)

volume integral: you can compute a variety of volume integrals of a chosen field variable.

– Volume: computes the total volume of the selected zones as a summation of the individual cell volumes.

(.)

– Sum: computes the sum of a chosen field variable over the selected zones.

(.)

– Volume Integral: is calculated by summing the product of cell volume and the selected field variable

over the selected zones.

(.)

– Volume-Weighted Average: is computed by dividing the volume integral of a selected field variable

(Equation . (p. )) by the total volume of the selected zones.

(.)

– Volume Variance: is the volume-weighted integral of the square of the deviation from the volume-

weighted average (Equation . (p. )), divided by the total volume of the selected zone.

(.)

– Mass Integral: is computed by summing the product of density, cell volume, and the chosen field variable.

(.)

– Mass: is computed by summing the product of cell density and cell volume.

(.)

– Mass-Weighted Average: is computed by dividing the Mass Integral of the chosen field variable (Equa-

tion . (p. )) by the total Mass (Equation . (p. )).

(.)

– Mass Variance: is computed as the mass-weighted summation of the square of the deviation of the

chosen field variable from its mass-weighted average (Equation . (p. )) divided by the total mass

(.)

The volume integrals listed above can be computed for the following field variables:

– Pressure

– Total Pressure

– Temperature (when adjoint energy is enabled)

– Total temperature (when adjoint energy is enabled)

– Velocity

– Velocity Magnitude

– Vorticity

– Vorticity Magnitude

– Turbulence Production:

– Velocity

... General Operations

Several operations are available to combine observables in various ways, if needed, to make a wide

variety of compound observables. The following operations are available:

ratio of two quantities

product of two quantities

linear combination of

quantities

, with constant coefficients

raised to various

powers

, plus a constant offset .

(.)

arithmetic average of

(.)

mean variance of

(.)

unary operation (sin, cosine, and so on) on observable value :

–

–

–

–

–

–

–

–

–

– ln

– log10

... Discrete Versus Continuous Adjoint Solver

When an adjoint solver is developed there is a key design decision that is made regarding the imple-

mentation, namely whether to use a continuous or a discrete approach. Both approaches are intended

to compute the same sensitivity data—however, the approaches are remarkably different.

While a user of the adjoint solver may experience no particular difference in workflow for the two

separate solver types, it is important to be aware that there are two primary classes of adjoint solver

and the approach chosen can have implications for the accuracy of the results.

A continuous adjoint solver relies heavily on mathematical properties of the partial-differential equations

that define the physics of the problem. In this case those equations are the Navier-Stokes equations.

With this approach an adjoint partial differential equation set is formulated explicitly and is accompanied

by adjoint boundary conditions that are also derived mathematically. Only after this derivation is

complete can the adjoint partial differential equations be discretized and solved, often with extensive

re-use of existing solver machinery. This class of solver was implemented by ANSYS Fluent as a research

effort.

Such a solver has the benefit that it is decoupled largely from the original flow solver. They share only

the fact that they are based on the Navier-Stokes equations. The process of discretizing and solving

the partial differential equations in each case could in principle be very different indeed. While this

flexibility may be appealing it can also be the downfall of the approach. Inconsistencies in modeling,

discretization and solution approaches can pollute the sensitivity information significantly, especially

for problems with wall functions and complex engineering configurations such as those of interest to

ANSYS Fluent users.

The continuous adjoint approach can be effective for some classes of problems. However, until there

is a significant advance in handling some key challenges, ANSYS Inc. has concluded that it is an unsuit-

able approach for meeting the needs of our broad client base for the classes of problems of interest

to them.

A discrete adjoint solver is based not on the form of the partial differential equations governing the

flow, but the particular discretized form of the equations used in the flow solver itself. The sensitivity

of the discretized equations forms the basis for the sensitivity calculation. In this approach the adjoint

solver is much more tightly tied to the specific implementation of the original flow solver. This has

been observed to yield sensitivity data that provides valuable engineering guidance for the classes of

problem of interest to ANSYS Fluent users, including problems with wall functions.

For the above reasons, the discrete adjoint approach has been adopted for the ANSYS Fluent adjoint

solver.

... Discrete Adjoint Solver Overview

As discussed in the previous section, a discrete adjoint approach to solving the adjoint problem has

been adopted, since it is believed to provide the most useful engineering sensitivity data for the classes

of problems of interest to ANSYS clients.

An adjoint method can be used to compute the derivative of an observation of interest for the fluid

system with respect to all the user-specified parameters, with any changes that arise in the flow variables

themselves eliminated. There are three key ingredients to consider when developing the method:

. All of the user-specified inputs:

All values set by a user in the boundary condition panels for each boundary in the problem.

The computational mesh. More specifically the locations of the nodes of the mesh and how they define

the edges, faces, and ultimately the cells used in the finite-volume computation.This includes both

interior as well as boundary nodes.

Material properties.

Model parameters such as model coefficients for turbulence models.

Note that the settings that define the problem are being distinguished from settings that define

how the solution advancement is to be performed to converge the problem. Only the former are

of interest here. For the sake of clarity, let us denote the vector of all of the values in the list by .

These are considered to be the control variables for the problem, that is, the variables that a user

can set explicitly that affect the solution.

It is worth noting that the topological definition of the mesh is fixed—it is not considered to be a

control variable here. The effect of collapsing cells or remeshing on the flow solution is not address-

able without further development in view of the discrete changes that are implied. This topic is

beyond the scope of the current document.

. The governing equations for the fluid system:

The main effort in a flow computation is in the determination of the flow state, namely the velocity,

pressure, density and possibly other fluid-related variables. For a cell-centered finite-volume scheme,

the flow state is defined at the cell centroids by a vector of real values. In the simplest case these

values are the pressure and flow velocity components. Let the vector of the variables in the

th

cell be denoted here by

.

At convergence the flow variables satisfy

(.)

where

is the number of cells in the problem, and there are  conditions on each cell. This ex-

pression is a compact way of denoting conservation of mass and momentum and other constraints.

. The engineering observation of interest:

Let

(.)

denote a scalar of interest that depends both on the flow state and perhaps directly on the control

variables. It is assumed that the observable is differentiable with respect to both the flow and the

controls. The inclusion of the control variables here is essential since in many cases the mesh

geometry is included directly in the evaluation of the observable. For example, the evaluation of

the force on a boundary involves the wall normal and face areas, which change when mesh nodes

are moved.

The goal is to determine the sensitivity of the observation with respect to the user-specified control

variables. What makes defining this relationship more challenging is the fact that changing the user

inputs changes the flow, which indirectly changes the engineering observation. The adjoint method

has a specific role in managing this chain of influences by providing a mechanism for eliminating the

specific changes that happen in the flow whenever the inputs change.

If a variation

is introduced into the control variables then a linearization of the governing equations

(Equation . (p. )) shows that the variations in the flow state

must satisfy

(.)

where there is an implied summation over  and , and

denotes that the flow solution is held constant

while the derivative is taken.

Meanwhile, if both the control variables and the flow state change, then the observation will change:

(.)

The particular way in which the flow responds to the changes in the control variables can be computed

using (Equation . (p. )) only after specific changes,

, have been chosen. It is prohibitive to

consider solving (Equation . (p. )) for more than a handful of prescribed changes

because

of the excessive computing time that would be needed. However, when redesigning the shape of

because

parts of a system there may be pressure to explore a large number of candidate modifications. This

conflict is reconciled by eliminating the variations of the flow solution from the expression (Equa-

tion . (p. )) and producing an explicit relationship between changes in the control variables

and the observation of interest.

This is accomplished by taking a weighted linear combination of the linearized governing equations

(Equation . (p. )) in a very particular way. A set of adjoint variables

is introduced with a one-

to-one correspondence with the governing equations (Equation . (p. )). This results in a relation-

ship

(.)

The term in square brackets on the left is now matched to the coefficient for the variation in the flow

in (Equation . (p. )) in order to define values for the adjoint variables:

(.)

These are the discrete adjoint equations, and the solution of this system that is the primary goal for

the adjoint solver. It is important to recognize that these equations have not been derived. They are

defined in this way with a specific goal in mind—the elimination from (Equation . (p. )) of the

perturbations to the flow field as shown below:

(.)

Note the use of Equation . (p. ) and Equation . (p. ) in the derivation of Equa-

tion . (p. ). The flow perturbation has now been eliminated from the expression, yielding a

direct relation between the control variables and the observable of interest.

There are several important observations to be made about (Equation . (p. )):

The dimension of the problem to be solved is the same as the original flow problem, although the adjoint

problem is linear.

While the adjoint solution may be considered strictly as a vector of numeric values, experience with the

continuous adjoint provides guidance on how the adjoint solution can be interpreted.The vector of weights

associated with the components of the residual of the momentum equation in each cell is termed the adjoint

velocity.The adjoint value associated with the residual of the continuity equation is termed the adjoint

pressure.

The right hand side is defined purely on the basis of the observable that is of interest.

The matrix on the left hand side is the transpose of the Jacobian of the governing system of equations

(Equation . (p. )).This seemingly innocent transposition has a very dramatic impact on how the

adjoint system is solved.This will be discussed below.

The adjoint equations are defined by the current state of the flow, and the specific physics that is employed

in the modeling. Each adjoint solution is specific to the flow state.

At first glance it appears that solving the adjoint problem may be straightforward. After all it simply

involves setting-up and solving a linear (albeit large) system of equations. In practice both steps can

represent a significant challenge, especially when the problem is large.

The evaluation of the residuals of the flow equations is an integral part of the pre-existing ANSYS

Fluent flow solvers. However, it is necessary to compute the Jacobian of the system

and

and

then transpose it, or at the very least to be able to make a matrix-free transpose matrix-vector product

with the adjoint solution. There are several technical approaches to accomplishing this task whose

description goes beyond the scope of this document. Suffice to say that it is not trivial to encode this

functionality, but that it has been done successfully here.

For the present implementation, a pre-conditioned iterative scheme, based on pseudo-time marching,

is adopted to solve the adjoint system. The equations that define the advancement process can be

written as

(.)

where

is a local time step size based on the local flow conditions,

is a user-specified CFL

number. The matrix

is a simplified form of the system Jacobian that is amenable to solution using

the AMG linear solver that is the workhorse of the conventional flow solver. The preconditioning

matrix

is a diagonal matrix. Artificial compressibility is introduced on the adjoint continuity equation

to aid in the relaxation of the adjoint pressure field.

The correction

is under-relaxed and added to the adjoint solution

and the process repeated

until the right hand side is adequately small.

... Adjoint Solver Stabilization

When applied to problems with large cell counts and complex geometry, adjoint solvers sometimes

experience stability issues. These instabilities can be associated with small scale unsteadiness in the

flow field and/or strong shear, and tend to be restricted to small and isolated regions of the flow domain.

Despite the spatial localization of these instabilities, the linearity of the adjoint problem provides no

intrinsic limit on their growth during solution advancement. Their presence, if not handled, can disrupt

the entire adjoint calculation despite the problem occurring in sometimes just a few cells. A stabilized

solution scheme will be required to obtain adjoint solutions for problems at high Reynolds number in

which there is strong shear and/or complex geometry.

Four stabilization schemes are available in Fluent in order to overcome these stability difficulties when

larger cases are being solved. You can choose to apply one of them at all times, or use a blended

strategy where up to two different schemes are used at different points in the solution. The stabilization

schemes are designed to intervene only when the standard advancement scheme is experiencing in-

Dissipation scheme

The dissipation scheme provides stabilization for the solution advancement of the adjoint solution by

introducing nonlinear damping strategically into the calculation domain.The strategy is intended to

provide minimal intervention in order to damp the growth of instabilities that lead to adjoint solution

divergence. A marker is tracked, based on the state of the adjoint solution, and damping is applied directly

to the adjoint solution in regions where the marker becomes large.

Unlike the modal, spatial, and residual minimization schemes, the dissipation scheme can affect

the adjoint solution slightly. In general, the spatial order of the damping is chosen to be one order

larger than the adjoint calculation order. This means that the formal order of accuracy of the adjoint

solver is unaffected by the addition of the dissipation scheme. In practice, regions of intense dis-

sipation can appear for some cases which may result in isolated spots and/or streaks in the solution

on surfaces. However, the scale of these solution features is such that they are often easily smoothed

during postprocessing to generate design changes.

Residual minimization scheme

The residual minimization scheme uses a GMRES-like scheme to approximate the solution by the

vectors in a Krylov subspace with minimal residual. The overall adjoint residual is guaranteed to

decrease. This is a unique benefit compared to the other available schemes. Note that this scheme

is expensive with regard to memory. When it is enabled, each main iteration consists of multiple

sub-iterations, where one sub-iteration is equivalent to one normal adjoint iteration.

Spatial scheme

The spatial scheme operates by identifying parts of the domain where unstable growth is occurring and

applying a more direct and stable solution procedure in those regions.

Modal scheme

The modal scheme involves a process of identifying the particular details of the unstable growth patterns

or modes.These patterns are localized in space and they are used to split the solution into parts that have

stable and unstable characteristics when advanced.The stable part is advanced as usual, while the algorithm

is designed now to compensate for the unstable part so that the overall calculation is stabilized.

The emergence of the unstable patterns can happen at any time during the adjoint calculation

and the total number of unstable patterns is case-dependent. Having  to  unstable modes

present would not be considered unusual. Large cases may have many more. As a general trend,

the most rapidly-growing unstable patterns appear often within a few iterations with more slowly-

growing modes appearing later in the calculation. The unstable patterns are handled as they appear.

Some additional computational overhead is associated with the stabilization schemes. In general, the

dissipation scheme is the least resource-intensive of the four schemes.

For information about using the stabilization schemes, refer to Stabilization Strategies, Schemes, and

Settings (p. ).

... Solution-Based Adaption

An adjoint solution provides guidance on where best to adapt a computational mesh in order to resolve

quantities of engineering interest.

Once the governing equations for the system (Equation . (p. )) have been converged there re-

mains a discretization error,

, such that

(.)

While specific estimates for this discretization error may be tricky to define, it is often estimated to be

, where  is the local grid size, and  is the order of the discretization scheme. That is,

for

a first-order scheme and

for a second order scheme. Alternatively,

can be considered to be the

residual associated with a solution that is not converged fully.

The correction to the flow field,

, that compensates for this inhomogeneity is given by

(.)

(.)

from which it follows quickly that

(.)

This simple expression provides an estimate of the effect of the presence of

on the observation,

.

The presence of discretization errors, or lack of convergence, on the engineering quantity of interest

is assessed by weighting the inhomogeneous term by the local adjoint solution. It is clear that even

in regions of the domain where the residuals or discretization errors are small, an accompanying adjoint

velocity or pressure that is large in magnitude implies that there may be a significant source of error

in the observable. A finer mesh in regions where the adjoint is large will reduce the influence of dis-

cretization errors that may adversely affect the engineering result of interest. In practice, adapting cells

which have large magnitude adjoint velocity and/or adjoint pressure will achieve this goal.

... Using The Data To Improve A Design

Adjoint sensitivity data can be used to guide how to modify a system in order to improve the perform-

ance. The observable of interest can be made larger or smaller, depending upon the engineering goal.

A common strategy for deciding how to modify the system is based on the gradient algorithm. The

underlying principle is quite simply that modifying a system in a manner to which it is most sensitive

maximizes the effect of the change. The change to a control variable is made in proportion to the

sensitivity of the value of interest with respect to that control variable.

Denote the sensitivity of the cost with respect to shape by

(.)

where

is the

(.)

where

is the

th coordinate of the

th node in the mesh. Here

is a notation for the subset of

the control variables

for the system that correspond to mesh node positions. Then an adjustment

(.)

will provide the maximum adjustment to  for given

norm of

, where  is an arbitrary scaling

factor. Note that  can be picked to be positive or negative depending upon whether  is to be in-

creased or decreased respectively. This is essentially a statement of the method of steepest descent.

Furthermore, the change is estimated to first order to be

(.)

For a sufficiently small adjustment, the change to the observation will strictly have the same sign as

the scaling factor , provided the gradient is not identically zero.

In regions where the sensitivity is high, small adjustments to the shape will have a large effect on the

observable. This corresponds directly with the idea of engineering robustness. If a configuration shows

high sensitivities, then the performance will likely be subject to large performance variations if there

are manufacturing inconsistencies. For a robust design, the goal is to have the sensitivity be tolerably

small.

In practical cases the field

can be noisy, especially for large, turbulent flow problems. If the

noisy field is used directly to modify a boundary shape using (Equation . (p. )), then the modified

surface can have many inflections. This is not helpful for engineering design work. In the next section,

the use of mesh morphing technology not only to smooth the sensitivity field, but also to provide

smooth boundary and interior mesh deformation, is described.

.... Smoothing and Mesh Morphing

As has been noted, for typical engineering problems, the shape sensitivity field can have smoothness

properties that are not adequate to define a shape modification. Mesh morphing technology is used

here for both two- and three-dimensional systems in a two-fold role. The first role is as a smoother

for the surface sensitivity field. The second role is to provide smooth distortions not only of the

boundary mesh, but also the interior mesh. This approach is very appealing since it functions for ar-

bitrary mesh cell types.

A Cartesian or cylindrical region is defined such that it encompasses all or a part of the problem domain.

Only the mesh nodes that fall within this region may move as a result of the morphing operation.

In general, an optimization problem may include both free-form minimization or maximization of the

observable(s) and constraints that are localized in space. This requires approaches that can provide

a deformation field that is well-behaved and consistent with manufacturability requirements, while

still allowing locally sharper deformations where required to satisfy the imposed constraints. For the

adjoint solver, Fluent provides two different morphing techniques: one based on polynomials, and

another that uses direct interpolation. Note that these methods are based on different design spaces,

and so will produce different morphing results.

..... Polynomials-Based Approach

Note

For simplicity, the smoothing and morphing equations presented here are for the case

Note

of a 2D domain. The same approach is extended and used for 3D problems.

For the polynomials-based morphing approach, a local ( , ) coordinate system is defined, where

and

. A regular array of

control points is then distributed in the control

volume. The motion of the mesh at any point in the domain is determined by the movement of the

control points. Bernstein polynomials and B-splines are used to map the control point motions to

the computational mesh nodes.

The

th Bernstein polynomial of degree  is:

(.)

The

th B-spline of degree  is the non-periodic B-spline that uses a knot-vector,

, where:

(.)

The value of the B-spline is defined recursively as:

(.)

Depending on the degree of the B-spline, the function is zero on some portion of the unit interval.

This is in contrast to the Bernstein polynomials that are strictly non-zero everywhere on the unit in-

terval.

Let

denote the

th mesh node, and let

denote the change in the pos-

ition of the node due to the morphing process. Let

denote the displacement of the

th

control point associated with the Bernstein polynomials in the

th coordinate direction, and let

th control point associated with the B-splines. If

denotes

the position of the

th mesh node, then the displacement of the node is defined by the superposition:

(.)

The control-point movement for the Bernstein polynomials controls the large-scale smooth deform-

ation, while the control-point movement for the B-splines controls fine-scale motions.

..... Direct Interpolation Method

In the direct interpolation method, the deformation of the interior mesh can be viewed as a projection

of the deformation from the boundary into the interior. The displacement of the interior mesh is

calculated as a weighted average of all boundary node displacement:

(.)

where

and

are the interior and boundary node displacements respectively,

is the

weighting function, and

is the distance between the i th and j th nodes.

When deciding which morphing method to choose, consider the following advantages of the direct

interpolation method compared to the polynomials-based approach:

It can handle design conditions better than the polynomials-based approach.

The design tool converges faster with the direct interpolation method: it converges with one iteration

for most design conditions.

Setting up the direct interpolation method is much simpler, as the following controls do not need to be

defined: most of the numerics settings, the freeform scaling scheme, the freeform scale factor, and the

number of control points.

The design conditions are satisfied exactly, even without applying strict conditions.

While the direct interpolation method has significant advantages, it also has the following limitations:

The interior mesh quality may not be as good as that produced by the polynomials-based approach

(though you may be able to mitigate this by using the Improve Mesh dialog box). Boundary zones are

also more at risk: they may cross / penetrate themselves or other boundary zones, which may or may

not generate a warning about cells with negative volumes; as a result, you must visually review the mesh

node changes, and reduce the target changes as needed.

Non-conformal interfaces should not undergo free deformation, as the morphing may move the two

sides apart.

Some region conditions are not supported, such as invariance, symmetry of motion, and region boundary

continuity.

This section describes the process for loading the adjoint solver module, as well as setting up, running,

and postprocessing the adjoint solutions. This section also demonstrates how the adjoint solution can

guide the modification of the boundary shapes.

The typical use of the adjoint solver involves the following steps (though not all of these may be neces-

sary for every workflow):

. Load or compute a conventional flow solution.

. Specify the observable(s) of interest.

. Set the adjoint solver controls.

. Set the adjoint solver monitors and convergence criteria.

. Initialize the adjoint solution and iterate to convergence.

. Postprocess the adjoint solution to extract the sensitivity of the observable with respect to the boundary

condition settings and the shape of the geometry.

. Set up the Design Tool and calculate the optimal design change.

. Modify the boundary shapes based on shape-sensitivity data and recompute the flow solution. The

former can be done through the Design Tool, whereas multiple iterations of both the former and

the latter can be performed by the Gradient-Based Optimizer.

This section provides information about using the ANSYS Fluent adjoint solver in the following sections:

... Model Considerations for Using Adjoint Solver

... Defining Observables

... Solving the Adjoint

... Postprocessing of Adjoint Solutions

... Modifying the Geometry Using the Design Tool

... Using the Gradient-Based Optimizer

In addition, see the Fluent Tutorials for more information about using the adjoint solver. (To access tu-

torials and their input files, go to the tutorials area of the customer site.)

The current adjoint solver implementation provides basic adjoint solutions that accompany a conven-

tionally-computed flow solution provided certain criteria are met.

.... Basic Assumptions and Consistency Checks

.... User-Defined Sources

The adjoint solver is implemented on the following basis:

The flow state is for a steady single-phase flow, or ideal gas, that is either laminar or turbulent.

For turbulent flows, a frozen turbulence assumption is made, in which the effect of changes to the state

of the turbulence is not taken into account when computing sensitivities.

For turbulent flows, the k-ε and k-ω models are supported.

For moving (that is, non-inertial) reference frame problems, the single reference frame (SRF) and

multiple reference frame (MRF) approaches are supported (as long as the absolute velocity formu-

lation is used), while the mixing plane model (MPM) is not. Note that for the MRF approach, the

adjoint solver does not support having a zone with a frame of motion that is relative to an already

moving reference frame.

Solid zones are supported, as long as they do not use a moving reference frame approach.

By default, the adjoint solver uses spatial discretization methods that are chosen for stability. If

desired, you can select more accurate methods, as described in Using the Adjoint Solution Methods

The boundary conditions are only of the following types:

– Wall (not including thin walls or shells)

Using the Adjoint Solver

– Velocity inlet

– Mass-flow inlet

– Mass-flow outlet

– Pressure inlet

– Pressure outlet

– Pressure far-field

– Symmetry

– Rotational and translation periodic

Constant and user-defined sources are supported for the momentum and energy equations; for

details on the latter, see User-Defined Sources (p. ). Note that temperature dependency is not

taken into account with the adjoint solver.

It is important to note that these requirements are not strict conditions for the conventional flow

solver, but rather modeling limitations for the adjoint solver.

When the adjoint solver is initialized or an observable is evaluated, and before iterations are performed,

a series of checks is performed to determine the suitability of the existing flow solution for analysis

with the adjoint solver. Two types of message may appear:

Warning message: There are certain physics models and boundary condition types that are not explicitly

modeled in the adjoint solver, but their absence does not disallow you from proceeding with the calculation.

In this case, a warning message will be printed that explains the nature of the inconsistency.

Checking adjoint setup...

-- Warning: Model is active but not included in adjoint calculation: P1 radiation model Done

The adjoint solver will still run in this case but the quality of the adjoint solution data can be ex-

pected to be poorer as a result of the inconsistency. This is because in such cases the unsupported

settings will revert to corresponding supported settings for the adjoint solver. Though the calculation

will proceed, it is important to note that the results produced should be considered on this basis.

When reverting back to the fluid calculation, the original settings will be preserved and the modified

settings are not migrated onto the original case. The warning indicates that the setting change will

be made automatically and specifically for the adjoint solution.

Error message: There are some model and boundary conditions that are incompatible with the computation

of an adjoint solution with the current adjoint solver implementation. In this case, an explanatory error

message will be printed in the console window.

** Unable to proceed: Model is active but not compatible with adjoint calculation:

Transition SST turbulence model

Done

The adjoint solver will not run in this case and changes must be made manually to the settings

identified in the console before the solver can be run.

User-defined sources for the momentum and/or energy equations that are defined in compiled UDFs

can be accounted for in the application of the adjoint solver, provided that the source derivatives

with respect to flow variables and cell centroid coordinates are provided. This is achieved by creating

the source term UDF definition in the usual fashion, with the exception that a special UDF macro is

used, DEFINE_SOURCE_AE (The suffix _AE denotes Adjoint Enabled).

DEFINE_SOURCE_AE (name, c, t, dS, eqn)

UDF name

symbol name

Index that identifies cell on which the source

term is to be applied

cell_t c

Pointer to cell thread

Thread *t

Array that contains the derivative of the

source term with respect to the dependent

real dS[]

variable of the transport equation, as well as

the flow variables and cell centroid position

Equation number

int eqn

real

Consider a source that may depend on velocity, pressure, and cell-centroid coordinates:

where ,

, and

are the Cartesian velocity components in the cell,

is the pressure in the cell, and

are the cell centroid coordinates as defined by the C_CENTROID macro. If the source

strength depends on one or more of these quantities, then the derivatives of the source strength

with respect to those variables must be computed and filled in as entries to the dS[] array. In par-

ticular,

must be defined in the UDF if there is a dependency of the source upon them. The specification of

this derivative information is essential for sensitivities, including shape sensitivity, to be computed

correctly by the adjoint solver.

Defining an observable is a key initial step that must be performed for any adjoint calculation. The

observable is the quantity for which sensitivities are sought. Observables can be defined based on

flow variables, or as operations on other observables. For a list of the types of observables you can

define refer to General Observables (p. ) and General Operations (p. ). You can define multiple

observables, but only one observable at a time can be selected for the adjoint sensitivity calculation.

Observables are created and selected in the Adjoint Observables dialog box, which is accessed by

clicking Observable... in the Design ribbon tab (Adjoint-Based group box). (Figure . : Adjoint Ob-

servables Dialog Box (p. )).

Design → Adjoint-Based → Observable...

Figure . : Adjoint Observables Dialog Box

.... Creating New Observables

.... Editing Observable Definitions

.... Selecting an Observable for Sensitivity Calculation

You can create a new observable by clicking Manage... in the Adjoint Observables dialog box and

then Create... in the Manage Adjoint Observables dialog box.

In the Create New Observable dialog box (Figure . : Create New Observable Dialog Box (Observable

Types) (p. )) you can choose from several observable types and operation types. Various types of

observable quantities can be defined and each can be given a name. The available types of observables

are described in General Observables (p. ).

Figure . : Create New Observable Dialog Box (Observable Types)

Select Observable types and pick an observable from the list. Keep the default name, or use the

Name field to designate a different name for the observable of interest. Click OK to create the new

observable, or click Cancel to dismiss the dialog box without creating an observable.

You can also combine existing observables in various ways or apply unary operations to create a wide

variety of compound observables. The operations that you can apply to existing observables are de-

scribed in General Operations (p. ).

Figure . : Create New Observable Dialog Box (Operation Types)

Select Operation types and choose an operation from the list. Keep the default name, or use the

Once created, you must edit the definition of the new observable (Editing Observable Defini-

Once an observable is created, it appears in the Observables list. When you select an observable in

the Observables list, the Manage Adjoint Observables dialog box changes to expose various

properties that can be assigned for the selected observable.

Figure . : Manage Adjoint Observables Dialog Box

Once the observable properties are defined (Inputs for Observable Types (p. )), click Apply to apply

the settings and proceed to define other observables, or click OK in the Manage Adjoint Observables

dialog box to apply the settings and close the dialog box. Available observables are described in

General Observables (p. ).

Note

Note

It is permissible to leave observable definitions incomplete. The Manage Adjoint

Observables dialog box can be considered as a workspace for the definition and

manipulation of observables. Only those operations with complete definitions will

appear in the Adjoint Observables dialog box. Operations with undefined fields, or

operations that depend on themselves, will be excluded from the list of usable observ-

ables.

Inputs for Observable Types

The inputs for each type of observable are summarized below:

For a force observable:

. Select the walls that are to contribute to the force of interest in the Wall Zones list.

. Define the direction in which the force is to be computed by entering the components of this

direction in the X Component, Y Component, and Z Component (for 3D) fields.

For a moment of force observable:

. Select the X, Y, and Z (for 3D) components of the Moment Center.

. Select the X, Y, and Z (for 3D) components of the Moment Axis.

. Select a wall in the Wall Zones list.

For a swirl observable:

. Select the X, Y, and Z (for 3D) components of the Swirl Center.

. Select the X, Y, and Z (for 3D) components of the Swirl Axis.

. Select a fluid in the Fluid Zones list.

For a pressure-drop observable:

. Select the inlets and outlets between which the total pressure drop is to be computed using the

Inlets and Outlets lists.

For a fixed value observable, perform the following:

. Select the Value of the Constant.

For a surface-integral observable:

. Select the type of integral from the Integral Type drop-down list. Available integral types are

described in General Observables (p. ).

. Select a Surface and the corresponding Field Variable.

For a volume-integral observable:

. Select the type of integral from the Volume Integral Type drop-down list. Available integral

types are described in General Observables (p. ).

. Select the Field Variable of interest. If the chosen field variable is a vector quantity, you will need

to specify a Direction along which the field variable will be evaluated.

. Under Integration Domain, select whether to integrate over selected Zones, a Box Region,

or a Cell Register.

. Select the Zones for integration, enter the coordinates of the rectangular (in 2D) or hexa-

hedral (in 3D) integration region under Box Settings, or make a selection from the Cell

Register drop-down list.

For a ratio observable:

. Select an observable from the Numerator drop-down list to represent the numerator of the ratio.

. Select an observable from the Denominator drop-down list to represent the denominator of the

ratio.

For a product observable:

. Select two observables from the corresponding drop-down list that will be used to compute their

product.

For a linear combination observable:

. Under Linear Combination of powers, select a Constant value.

. Select the number of Components.

. For each component, select a corresponding Coefficient, an Observable, and a Power.

For an arithmetic average observable:

. Select observables from the corresponding Observable lists.

For a mean variance observable:

For a unary operation observable:

. Select an operation from the drop-down list (see General Observables (p. ) for a list of available

operators).

. Select an observable from the corresponding drop-down list upon which the unary operation is

to be applied.

You can select which observable to use for the sensitivity calculation in the list of Observable Names.

Note

Only one observable can be used in any one adjoint calculation. In the Adjoint Observ-

ables dialog box, the observable that is currently highlighted is the observable that will

be used in the sensitivity calculation.

Any observables that have been created but which are missing required inputs will not

appear in the list of Observable Names.

Clicking the Evaluate button computes the current value of the selected observable quantity and

prints the result in the console window. Clicking the Write... button provides the option to write the

result to a named file.

The Sensitivity Orientation determines the sign of the postprocessed sensitivities. For instance, if

you select Maximize then changes in the direction of positive sensitivities will increase the value of

the observable. A standard rule of thumb can be applied: if you want to improve the solution, then

follow the direction of the sensitivity vectors. Another standard rule of thumb can also be applied

for postprocessed scalars: if you want to improve the solution, then increase values where the sensit-

ivity is positive and/or decrease values where the sensitivity is negative.

Once an observable is defined as described in Defining Observables (p. ), the solution of the adjoint

for that observable can be computed based on the current flow solution. The steps for solving the

adjoint are similar to those for solving the flow and are detailed in the following sections:

.... Using the Adjoint Solution Methods Dialog Box

.... Using the Adjoint Solution Controls Dialog Box

....Working with Adjoint Residual Monitors

.... Running the Adjoint Calculation

You can specify the methods used for computing the adjoint solutions in the Adjoint Solution

Methods dialog box. To open the Adjoint Solution Methods dialog box, click Methods... in the

Design ribbon tab (Adjoint-Based group box).

Design → Adjoint-Based → Methods...

Figure . : Adjoint Solution Methods Dialog Box

The Adjoint Solution Methods dialog box shows a side-by-side comparison of the schemes used

for the flow solver and for the adjoint solver. Using the same scheme for the adjoint solution and the

flow solution yields the most accurate discrete derivative calculation when the adjoint solution is

converged. However, not all schemes used for the flow solver are supported for the adjoint solver.

In these cases an alternate adjoint scheme must be used. This does not typically lead to severe deteri-

oration of the adjoint results quality. Even if the same scheme is available for the adjoint solver this

is not always practical because stability may be reduced with some schemes. Therefore, you can use

the drop-down lists under Adjoint Solver to select alternate schemes as needed.

In some cases it may not be desirable to solve the energy adjoint even if energy is solved in the flow

solver. For example, consider an incompressible flow where the specified observable does not involve

thermal quantities. In this case the adjoint for the energy equation is identically zero, but its inclusion

would add an unnecessary numerical burden. You can disable the Adjoint Energy option to avoid

solving the energy adjoint.

If the primary flow is a compressible ideal gas, you can specify that the physics of the compressible

flow are modeled in the adjoint solver by enabling the Adjoint Ideal Gas option. Enabling this option

automatically enables the Adjoint Energy option as well. If the flow is not a compressible ideal gas,

it will be treated as being incompressible for the purposes of the adjoint calculation.

Clicking Default will set the spatial discretization methods for the adjoint solver to Green-Gauss Cell

Based for gradient, Standard for pressure, and First Order Upwind for momentum, which are chosen

for their stability. Clicking Best Match will attempt to match the adjoint schemes to the flow schemes

that should in general provide more accurate calculations at convergence. Where they cannot be

matched, the default scheme will be used.

The advancement of the adjoint solution to reach a converged solution is an essential part of the

analysis. The solution algorithm for the adjoint solver is similar to the coupled pressure-based solver

that is available for conventional flow computations in ANSYS Fluent.

By default, the adjoint solver advancement settings will be automatically adjusted during calculation

to encourage convergence, with initial values determined by the state of the flow solution. If needed,

you can adjust the advancement controls in the Adjoint Solution Controls dialog box.

To open the Adjoint Solution Controls dialog box, click Solver Controls... in the Design ribbon tab

(Adjoint-Based group box).

Design → Adjoint-Based → Solver Controls...

Controls

Solution-Based Controls Initialization

When enabled, the advancement controls are selected automatically when the adjoint solution is initialized

based on the state of the flow.

Stabilization Settings...

This button opens the Stabilized Scheme & Strategy Settings dialog box, which you can use to define

the stabilization strategy, scheme(s), and settings for the adjoint solution. For details, see Stabilization

Strategies, Schemes, and Settings (p. ).

Auto-Adjust Controls

When enabled, the convergence of the AMG solver and the adjoint residuals are monitored during

solution advancement. Based on the trends observed, the Courant number is automatically adjusted

to encourage reliable solution advancement and convergence. This is especially useful when a

new type of problem is being solved for which appropriate settings are not initially clear. You

can enable or disable Auto-Adjust Controls at any time during the solution.

The Courant number starts at the value you defined in the Advancement Controls group box

or the value determined by the Solution-Based Controls Initialization option. When the residual

minimization scheme is used, over the first two iterations the Courant number will be increased

as high as possible (while still allowing the AMG solver to converge), and will then remain un-

changed; for all other setups, the Courant number will be adjusted to ensure the AMG solver

converges, with the goal of reducing the AMG residuals at the rate of  order of magnitude over

iterations. Messages will appear as the calculation progresses indicating the adjustments that

are being made.

Show Advancement Controls

This option toggles the visibility of the various advancement controls for direct user specification.

Advancement Controls

contains the advancement controls.

Apply Preconditioning

Enables solution preconditioning.This is needed for most cases involving turbulent flow. If precon-

ditioning is enabled, additional controls are available.

A higher number corresponds to a more aggressive advancement of the computation at the risk of

instability. Disabling preconditioning corresponds to an infinite Courant number.

Artificial Compressibility

A nonzero value introduces artificial compressibility into the computation of the adjoint continuity

equation. A value of . or less is reasonable.

Flow Rate Courant Scaling , Energy Equation Scaling

These values should be larger than zero (default value is . for flow rate and  for energy). A

smaller value implies a less aggressive algorithm that encourages stability of the AMG linear solver.

contains the under-relaxation factors.

Adjoint Momentum , Adjoint Continuity , Adjoint Local Flow Rate , Adjoint Energy

Each of these can be set to a value between . to .. A higher value leads to a more aggressive

algorithm that is less likely to be stable. A value of . for each can be used for some simple cases

without difficulty.

Algebraic Multigrid

contains the algebraic multigrid controls.

Tolerance

The tolerance used for judging convergence.

Maximum Iterations

The maximum number of inner iterations of the AMG solver.

Show Iterations

If enabled, a more verbose iteration history is printed in the text console during iterations.The details

of the inner iteration can be useful when deciding on appropriate Courant Number, Artificial

Compressibility, and Flow Rate Courant Scaling. If many inner iterations are needed, or if the inner

iterations diverge, this signals that a reduction in Courant Number may be needed. Alternatively,

an increase in Artificial Compressibility or a reduction in the Flow Rate Courant Scaling may be

sufficient for the AMG iterations to converge.

..... Stabilization Strategies, Schemes, and Settings

For an overview of when stabilization is needed and descriptions of the available schemes, see Adjoint

Solver Stabilization (p. ). You can define a stabilization strategy in the Stabilized Scheme &

Strategy Settings dialog box, which is opened by clicking the Stabilization Settings... button in

the Adjoint Solution Controls dialog box.

Figure . : The Stabilized Scheme & Strategy Settings Dialog Box

Selecting None from the Type list in the Stabilization Strategy group box on the left allows you

to select a single stabilization method to be used throughout the calculation, or none at all. You

specify your preference using the Type list in the Stabilization Scheme group box on the right and

then define the scheme settings using controls below the list.

Alternatively, you can select Blended from the Type list in the Stabilization Strategy group box

on the left, so that either no scheme (None) or the Dissipation scheme is applied at the beginning

of the calculation, depending on your selection from the Scheme drop-down list in the 1st Scheme

group box; then a second scheme (the residual minimization scheme) is used for the remainder of

the calculation. If you enable the Auto Detection? option, the first scheme will be used until diver-

gence or slow convergence in the adjoint residual is detected; otherwise, you specify an explicit

number of Iterations to be run before switching to the second scheme. The latter can be useful for

cases that take a long time to diverge or show signs of slow convergence with the first scheme, as

you can force an early switch to the residual minimization scheme (which generally converges

quickly). You can also specify the maximum number of Iterations to allow for the 2nd Scheme, as

the residual minimization scheme can be expensive on a per iteration basis. Note that settings used

for the dissipation and residual minimization schemes are defined in the Stabilization Scheme

group box on the right, by selecting each scheme in turn (from the Type list), and then using the

controls below the list as described in the sections that follow.

Note

After your first calculation is complete, the second stabilization scheme will be used at

the start of all subsequent calculations, unless you click the Initialize Strategy button in

the Run Adjoint Calculation dialog box prior to calculating. Initializing the strategy is

recommended when there is an operation that will cause a residual jump (such as

morphing the mesh), as the first scheme can resolve some of the modes more efficiently.

When using the Blended strategy, note that you can use the Default button to revert any changes

you have made to the settings. You can also use the Complex Case button to use settings that are

more appropriate for complex cases that would benefit from the initial use of the dissipation scheme

to damp local diverging modes, before switching to the residual minimization scheme; note that for

some cases, you may need to increase the Iterations for the dissipation scheme or increase the

damping factor in the Stabilization Scheme group box (for example, to ) to allow the scheme

to fully damp the modes.

The Stabilization Scheme settings are described in the following sections:

...... Dissipation Scheme

...... Residual Minimization Scheme

...... Spatial Stabilization Scheme

...... Modal Stabilization Scheme

The dissipation scheme operates by introducing nonlinear damping strategically into the calculation

domain. The strategy is intended to provide minimal intervention in order to damp the growth of

instabilities that lead to adjoint solution divergence. A marker is tracked, based on the state of the

adjoint solution, and the damping is applied directly to the adjoint solution in regions where the

marker becomes large.

Figure . : The Dissipation Scheme Settings

After selecting Dissipation from the Type list, you can define the following settings:

Damping Factor

The overall level of dissipation is proportional to this value although the damping level is determined

ultimately through a nonlinear process.

Damping Relaxation

The damping relaxation can be used to control the rate at which the dissipation is updated as

the adjoint solution progresses. As you decrease the value from , the rate at which the dissipation

is updated is decreased.

Damping Order

The spatial order of the dissipation. A higher order leads to more intense and localized damping.This

can typically be set to be one order larger than the adjoint calculation spatial order.

Suppression

As part of the dissipation scheme, the growth of instabilities is stopped by the effect of the dis-

sipation; enabling the Suppression option ensures that these undesirable patterns will then also

decay as the calculation progresses.

Since the order of discretization of the dissipation scheme is usually set higher than the adjoint, the

formal order of accuracy of the adjoint solution is unaffected by the addition of dissipation. However,

regions of intense dissipation can appear for some cases when using this scheme. This can sometimes

appear as isolated spots and streaks in the adjoint solution on surfaces. The scale of these features

is such that they are often easily smoothed during postprocessing to generated design changes.

The residual minimization scheme operates by building a Krylov subspace and using it to build a

solution with minimum residual.

Figure . : The Residual Minimization Scheme Settings

After selecting Residual Minimization from the Type list, you can define the following settings:

Number of Modes

This specifies the number of modes in the Krylov subspace used to approximate the solution. Increasing

the number of modes will increase the convergence and reduce the final residual.The convergence

rate may increase sharply when the number of modes is larger than a certain threshold. Note that the

memory needed for this scheme is proportional to (number of adjoint equations) * (number of modes

+ number of recycled modes).You should ensure that you have enough memory for the value you

enter here; an estimation of the additional memory needed at the peak is printed in the console when

you click Apply.

Show Expert Controls

Enabling this option reveals the expert controls described below, so that you can adjust them from the

Number of Recycled Modes

This specifies the number of modes that are selected, stored, and used for the next iteration to speed

up the convergence.The default value is a quarter of the number of modes.

For the initial step of the residual minimization scheme, the number of sub-iterations is equal

to the number of modes; for later steps, it is the difference of the number of modes and the

number of recycled modes. Therefore, increasing the number of recycled modes will reduce the

number of sub-iterations for each main iteration; while this relation is straightforward, the effect

on the overall convergence ratio is not, as it is case dependent.

AMG Iterations

This specifies the fixed number of AMG iterations in each sub-iteration. Increasing the number may

improve the overall convergence, but it also increases the time for each sub-iteration.The residual

minimization scheme is unique in that it does not require the AMG solver to reduce the inner residual

by at least one order; it only requires that the AMG solver not be diverging. In fact, a more aggressive

setting of preconditioning may slow down the inner AMG convergence, but improve the overall outer

loop convergence. Such an improvement can be significant.

Note

The following tips can be helpful when using the residual minimization scheme:

It is highly recommended that you first run the adjoint solver without a stabilization

scheme until the adjoint residual starts to diverge, and then enable the residual minim-

ization scheme. The first run damps out many stable modes in the adjoint residual and

reduces the number of modes required in the residual minimization scheme. Note that

this can easily be done by selecting the Blended strategy in the Stabilization Strategy

group box.

The overall adjoint residual will be printed in the console.The residual should either decrease

monotonically or stall within each main iteration or between main iterations. If you do not

see such behavior, click the Initialize Stabilization button in the Run Adjoint Calculation

dialog box to initialize the scheme.

The spatial scheme operates by identifying parts of the domain where unstable growth is occurring

and applying a more stable scheme. The unstable mode tracking and handling is done in an auto-

mated manner. Several settings are exposed, but are recommended for expert users only.

To enable the spatial stabilization scheme and define the settings, use the following text command:

adjoint → controls → stabilization

The settings available for this scheme include the following. The first four settings relate to unstable

mode tracking and selection, while the next three provide options for the response once a mode is

identified.

Tracking History Length

defines the number of iterations that are employed in the unstable mode identification process. A range

between  and  may be chosen.The longer the tracking history, the better the quality of the identific-

Resolution Threshold

defines a threshold for the separation between modes based on their amplitudes. A value of . implies

that the second most-dominant mode must be . of the amplitude of the primary mode before an

unstable mode can be considered as being adequately resolved.

Coherence Threshold

defines a threshold that must be met for the closeness of the mode to pure exponential growth as the

iterations progress. A smaller number means that a tighter tolerance must be met before an unstable

mode is considered as having been identified.

Growth Threshold

defines the growth rate threshold for unstable modes that must be met before the algorithm responds

to the presence of the mode.The growth threshold defines the number of iterations that would have

to take place for the mode to grow by one order of magnitude.That is, a value of . signifies that a

mode that would grow one order of magnitude or more in  iterations will be handled. A negative

value for this threshold is not recommended as multiple stable modes may be tracked.

Maximum Number of Cells

defines a limit on the number of cells for which stabilization will be applied when an unstable mode is

located.

Mode Amplitude Cutoff

defines the fraction of the peak mode amplitude beyond which cells will be included for stabilization.

Solution Blending

defines an under-relaxation factor for blending the stabilized part of the scheme with the standard

advancement scheme. A default of . is chosen.The value should lie between  and .

Print Mode Information

(when enabled) leads to details of the unstable mode tracking process being printed in the console

window.The following is an example of what is printed when a mode is resolved partially:

Mode present> Growth :    .38166e-  Coherence  :    .27858e+

Resolution Threshold :    .00000e-  Resolution :    .32611e-

The following is an example of what is printed when a mode becomes more fully resolved:

Mode present> Growth :    .35318e-  Coherence  :    .84133e-

Resolution Threshold :    .00000e-  Resolution :    .75312e-

Growth Threshold     :    .60193e-  Growth     :    .35318e-

Coherence Threshold  :    .00000e-  Coherence  :    .84133e-

Local stabilization required: Instability detected in  cells

The final line only appears when a coherent and resolved instability has been identified success-

fully. Subsequently, the solution advancement algorithm automatically adjusts to eliminate this

unstable behavior.

Print Local Solve Residuals

(when enabled) leads to details of the residuals for the local solution process being printed in the

console window. An example of what is printed is given below:

Iter   Adjoint-continuity  Adjoint-xMom     Adjoint-yMom      Adjoint-Flowrate

....

.76334e-      .57503e-      .26984e-        .92618e-

Local (%)     . . . .

The percentage residual indicates the fraction of the total residual that is associated with the

local solution process.

The behavior of the modal scheme is as follows. As the calculation progresses the solution is mon-

itored for unstable growing patterns or modes as the adjoint solution is corrected by the primary

advancement algorithm. The first stage of the stabilization scheme involves a lightweight monitoring

process to screen for any unstable patterns. If the calculation is progressing in a stable manner there

is no indication even that the stabilization scheme is operating. If a candidate instability appears

then it is monitored. In the event that unstable behavior that cannot be handled by the primary

advancement scheme becomes evident a more intensive process is activated. Unstable patterns are

refined using a fixed point iteration scheme so that they can be handled cleanly and advanced in a

stable manner using an alternative to the primary advancement scheme.

To enable the modal stabilization scheme and define the settings, use the following text command:

The settings available for this scheme include the following:

controls the preliminary screening for growth. It defines the threshold for relative variance of growth

between iterations at which a more detailed search is activated. A smaller value will tend to delay the

activation of the more detailed search for unstable growth at the risk of allowing unstable growth to

continue for more iterations.

Max. Fixed Point Iterations

is the maximum number of iterations taken to refine the unstable pattern during the more detailed

search.

Mode Purity Threshold

is the tolerance for an acceptable unstable pattern. A smaller value will lead to a purer unstable mode

being identified.This may occur at the expense of a larger number of fixed point iterations. If the purity

threshold is not met after the maximum specified number of iterations then the unstable pattern is

rejected.

Conjugate Pair Threshold

rejected.

is the threshold for inclusion of a second unstable mode alongside a candidate mode, forming a con-

jugate pair.This corresponds to a pseudo-time-periodic instability, versus purely exponential growth.

Such instabilities can occur in some cases. Increasing this value will increase the occurrence of a second

mode being included.

is the largest number of cells allowed for an unstable pattern that will be handled by the stabilization

scheme.The problematic instabilities for an adjoint solver are often localized in space to a small number

of cells out of the entire flow domain. However, there can be transiently growing corrections to the

adjoint solution that masquerade as unstable patterns.This cell limit suppresses such false patterns

from consideration.

Mode Norm Cutoff

serves to identify the main body of an unstable pattern and exclude the peripheral spatial parts of the

mode that are of small amplitude. If the norm cutoff was set to zero, all unstable modes would involve

all cells in the domain.Therefore, reducing this value increases the number of cells that are included

in an unstable mode.

Regularization

acts to regularize the advancement of the unstable mode components.The stiffness of the adjoint

governing equations can give rise to difficulty in discerning the unstable pattern from nearby stable

patterns. Increasing the regularization tends to overcome this difficulty and adds stability to the calcu-

lation at the expense of potentially slower convergence.Valid values are between  and .

enables printing of stabilization information to the console.

When using the modal stabilization scheme, the following behavior can be observed:

When the primary advancement scheme is proceeding in a stable manner, the stabilization scheme

will remain idle and no output will be generated.

When a candidate unstable pattern appears it will be tracked and a message will appear with inform-

ation about the detected mode:

Mode growth:    .34390e+  Coherence:    .28546e-

In the above example, the message indicates that an unstable pattern that grows by more than %

in one iteration is present.The value of the Coherence corresponds to the variance in growth

between iterations.

When a candidate unstable pattern is identified that meets the coherence threshold, the secondary

refinement stage is activated:

Mode growth:    .35752e+  Coherence:    .95870e-

Growing pattern cell count:

Isolating new mode

Iteration:   Growth rate:    .42665e+   Residual:    .88196e-

Iteration:   Growth rate:    .41329e+   Residual:    .34600e-

Iteration:   Growth rate:    .41227e+   Residual:    .25348e-

New growing mode with  cells

If the growing pattern cell count exceeds Maximum Number of Cells the refinement procedure

is postponed. Likewise, if after refinement the number of cells involved exceeds the specified limit

the mode is rejected. Each iteration corresponds to a refinement of the unstable pattern.The adjoint

solution itself is not advanced during this process.The residual corresponds to the purity of the

mode and must eventually fall below the Mode Purity Threshold for the mode to be accepted.

A minimum of  iterations is taken so that the occurrence or absence of a conjugate pair can be

verified.

The presence of the sometimes violent unstable growth that can occur gives a jagged appearance

to the adjoint residual plots. However, the underlying trend of the residual plots should correspond

to a converging adjoint solution process.

The unstable patterns of solution advancement are specific to the flow solution, choice of discretiz-

ation schemes, and solution advancement controls for the adjoint solver. If any of these values

changes, then the unstable modal patterns must be recomputed so that the stabilization scheme

will function to full effect. In the event that any of these parameters is changed and the adjoint

solution is restarted a mode recalibration process will be initiated. It should be noted that if there

are many unstable modes that have been identified then this recalibration may take some time.

In contrast, the patterns of unstable growth are not specific to the observable that has been selected.

Given that there is computational effort needed to identify the instabilities, a separate initialization

process is available just for the unstable modal patterns. This allows the adjoint solution itself to be

initialized for a new observable while retaining the knowledge of how to stabilize the solution ad-

vancement. A much smoother path to solution for the second and subsequent observables is then

achieved.

achieved.

The progress of the iterations of the adjoint solver and the monitoring of the convergence is controlled

in the Adjoint Residual Monitors dialog box. This dialog box is accessed by clicking Monitors... in

the Design ribbon tab (Adjoint-Based group box).

Design → Adjoint-Based → Monitors...

Figure . : Adjoint Residual Monitors Dialog Box

The steps to define the monitor behavior are as follows:

. Decide whether or not the residuals are to be printed in the console by setting the Print to Console

check box as desired.

. Decide whether or not the residuals are to be plotted in the main window by setting the Plot check box

as desired.

. Set the ID of the window in which the adjoint residuals are to appear in the Window field.

. Set how many iterations are to be shown in the residual curves that are plotted in the Iterations to Plot

field.

. Enable and/or disable those values that are to be used as criteria for convergence, and set the Criteria

in each case.The options are to test the residuals for the following equations: Adjoint continuity, Adjoint

velocity, Adjoint local flow rate, and/or Adjoint energy.

Click the OK or Apply buttons to confirm that the settings are acceptable. Clicking Plot will cause

existing adjoint residuals to be plotted in the main graphics window.

Initialization and execution of the adjoint solver is accomplished in the Run Adjoint Calculation

dialog box. This dialog box is accessed by clicking Calculate... in the Design ribbon tab (Adjoint-

Based group box).

Design → Adjoint-Based → Calculate...

Figure . : Run Adjoint Calculation Dialog Box

The function of this dialog box is as follows:

sets the value of the adjoint velocity and pressure to zero everywhere in the problem domain.

Initialize Strategy

initializes the stabilization strategy, such that the first stabilization scheme is used at the start of the next

calculation rather than continuing to use the second stabilization scheme.This button is only available

when the blended stabilization strategy is used. For details, see Stabilization Strategies, Schemes, and

Initialize Stabilization

clears all of the unstable modes that have been identified in calculations using the stabilization scheme,

but leaves the adjoint solution unchanged.This button is only available when the residual minimization

scheme or modal scheme is enabled.

Number of Iterations

sets the number of iterations for the calculation. Note that if you are using a blended stabilization strategy,

the calculation may end sooner if the total of the iterations you specified in the Stabilized Scheme &

Strategy Settings dialog box (described in Stabilization Strategies, Schemes, and Settings (p. )) is

less than the value you enter here.

Calculate

advances the adjoint solver by the Number of Iterations specified in the adjacent field.

Depending on the monitor settings, the residuals may be printed in the console and/or plotted in

the main graphics window.

Adjoint solution data can be postprocessed so that it provides both qualitative and quantitative views

of the effect of many types of change that may be imposed on a system. While shape changes are

often of particular interest there is a very rich data set, one as large as the original flow field, available

for exploration. Postprocessing tools are provided with the intention of permitting the adjoint data to

be mined in such a way that it provides useful supporting information for an engineer who is making

design decisions for a system, or has questions about the reliability of the original flow calculation.

Since the ANSYS Fluent adjoint solver is a discrete adjoint solver, the primitive adjoint solution data

provides sensitivity to changes cell-wise for the computational mesh. Normalization of these results

by the cell volume provides a mesh-independent view into the data set.

Information regarding postprocessing the adjoint solutions can be found in the following sections:

.... Field Data

.... Scalar Data

Adjoint solution data can be postprocessed using standard ANSYS Fluent postprocessing tools including

contours, vectors, xy-plots, histograms, and surface and volume integrals.

In the Contours dialog box, under Sensitivities..., you can find the following fields:

This field is the magnitude of the adjoint velocity primitive field.This field can be interpreted as the

magnitude of the sensitivity of the observable to body force per unit volume. It can be used to

identify regions in the domain where small changes to the momentum balance in the flow can have

a large or small effect on the observable.This field is often observed to be large, for example, up-

stream of a body for which drag sensitivity is of interest, with the field diminishing in the upstream

direction.This indicates the interference effect for an object positioned at various locations upstream

of the object of interest.

Sensitivity to Body Force X-Component (Cell Values), Sensitivity to Body Force Y-Component

(Cell Values), and Sensitivity to Body Force Z-Component (Cell Values)

These are the components of the adjoint velocity primitive field.These fields can be interpreted as

the magnitude of the sensitivity of the observable to components of a body force per unit volume.

Consider a body force distribution, expressed as a force per unit volume.The volume integral of

the vector product of that distribution with the components of this field gives a first-order estimate

This field is the primitive adjoint pressure field.This field can be interpreted as the sensitivity of the

observable with respect to mass sources or sinks in the domain. Consider a mass source / sink dis-

tribution, expressed as mass flow rate per unit volume.The volume integral of that distribution,

weighted by the local value of this field, gives the effect of the sources / sinks on the observation.

When plotted on a boundary, this field indicates the effect of the addition or removal of fluid from

the domain upon the quantity of interest. It is important to note that in this scenario the effect of

the momentum of the fluid that is added or removed is not taken into account.The boundary velocity

sensitivity should be plotted if that effect is also of interest.

This field is available when the energy adjoint equation is solved and is the primitive adjoint tem-

perature field. It can be interpreted as the sensitivity of the observable with respect to the thermal

This field is available when the adjoint dissipation stabilization scheme is enabled and shows the

location and amount of the nonlinear damping that has been introduced to damp the growth of

instabilities that lead to adjoint solution divergence.

This field shows the sensitivity of the quantity of interest to variations in the turbulent effective

viscosity for a turbulent problem, or the laminar viscosity in a laminar case.The sensitivity is normal-

ized by the cell volume to account for cell size variations in the mesh.

This field is the magnitude of the sensitivity of the observable with respect to a deformation applied

to the mesh (both boundary and interior mesh).When plotted on the surface of a body the locations

where this quantity is large indicates where small changes to the surface shape can have a large

effect on the observable of interest. If the shape sensitivity magnitude is small then the effect of

shape changes in this region can be expected to have a small effect on the observable of interest.

When viewing this field, it is often observed that the magnitude varies by many orders of magnitude.

Contour plots will clearly draw attention to regions with the highest sensitivity (often sharp edges

and corners). However, it should be remembered that a relatively small surface movement that is

distributed over a large area can have a cumulative effect that is large.

This field shows the normal component of the shape sensitivity. A positive value indicates an orient-

ation directed into the domain, while a negative value indicates that the shape sensitivity is oriented

outwards from the domain.This field eliminates the component of the vector shape sensitivity field

that lies in the plane of the wall.

This field shows the normal component of the optimal displacement computed from the adjoint

solution.This field is defined only for portions of walls lying within the control-volume specified for

morphing.The size of the optimal displacement is determined by the scale factor that is chosen for

the morphing. A positive value of displacement indicates that the surface will be displaced into the

flow domain, whereas a negative value of displacement corresponds to wall movement outwards

from the flow domain.This field eliminates the component of the optimal displacement vector that

lies in the plane of the wall.

In view of the large range of values possible for the shape sensitivity magnitude, a convenience

function that plots

of the magnitude is provided.This allows the importance of the surfaces

in a domain to be ranked more easily based on how they affect the observation of interest when

they are reshaped.

Shape Sensitivity X-Component, Shape Sensitivity Y-Component, and Shape Sensitivity Z-Com-

ponent (in 3D) fields

These fields are the individual components of the sensitivity of the observable of interest with respect

to the mesh node locations. It is plotted as cell data and is computed as the average of the nodal

sensitivities for a given cell, divided by the cell volume. Note that for this discrete adjoint solver the

sensitivity of the result with respect to node locations both on and off boundaries is computed.The

normalization by cell volume indicates that the fields that are plotted are the weighting factors for

a continuous spatial deformation field. (Note that the nodal sensitivity data itself is used when mesh

morphing is performed, and predictions about the effect of shape changes are made.)

Sensitivity to Boundary X-Velocity, Sensitivity to Boundary Y-Velocity, and Sensitivity to

Boundary Z-Velocity (in 3D) fields

These fields are defined on those boundaries where a user-specification of a boundary velocity is

made for the original flow calculation.This includes no-slip walls.The field shows how sensitive the

observable of interest is to changes in the boundary velocity at any point. It is interesting to note

that even though the original boundary condition specification may be for a uniform velocity on

the domain boundary, the effect of a non-uniform velocity perturbation is available.The effect of

any specific boundary velocity change can be estimated as an integral of the vector product of the

change to the velocity with the plotted sensitivity field. A plot of this quantity on a velocity inlet,

for example, can be very useful for assessing whether or not the inlet is positioned too close to key

parts of the system.That is, it addresses the question of whether or not the flow domain is too small

to achieve a successful computation of the performance measure of interest.Viewing this field will

also indicate whether or not the assumption of a uniform inflow is adequate.

This field is defined on boundaries where there is a user-specified pressure as part of a boundary

condition, such as on a pressure outlet.The field shows the sensitivity of the observation of interest

to variations in the boundary pressure across the flow boundary. It is interesting to note that even

though the original boundary condition specification may be for a uniform pressure on the domain

boundary pressure change can be estimated as an integral of the product of the change to the

pressure with the plotted sensitivity field.Viewing this field will also indicate whether or not the

assumption of a uniform pressure is adequate for the simulation.

This field is available when the energy adjoint equation is solved and is defined on boundaries

where a temperature boundary condition is applied. This includes walls, velocity inlets, mass-

flow inlets, pressure inlets, pressure far-field boundaries, and pressure outlets where a backflow

temperature may be specified. The field shows the sensitivity of the observation of interest

to variations in the boundary temperature across the boundaries. Note that even if the ori-

ginal boundary condition specification is for a uniform temperature on the boundary, the

effect of a non-uniform temperature perturbation is available. The effect of any specific

boundary temperature change can be estimated as an integral of the product of the change

to the temperature with the plotted sensitivity field. This field can be used to indicate

whether or not the assumption of a uniform temperature is adequate for the simulation.

This field is available when the adjoint energy equation is solved and is defined on walls where a

heat flux boundary condition is imposed.The field shows the sensitivity of the observation of interest

to variations in the boundary heat flux through the wall. Its properties are analogous to those of

Sensitivity to Boundary Temperature.

This field is provided as a convenient tool for identifying portions of the flow domain where the

introduction of blockages or obstructions in the flow can affect the observation of interest. Consider

a blockage in the flow that generates a reaction force on the flow that is proportional to the local

flow speed, and acting in the opposite direction to the local flow:

coefficient for the reaction force.The local contribution of this force on the observation of interest

is determined by the vector product of this force with the adjoint velocity field.The flow blockage

field that is plotted is

, namely the negative of the vector product of the flow velocity and the

adjoint velocity (Cell Value).

This field, intended for expert users who are using the Spatial Stabilization Scheme (p. ), can be

plotted to identify those portions of the flow domain where the stabilized adjoint solution advance-

ment scheme is applied. It is preferable to plot this with the Node Values disabled in the Contours

dialog box. In this case, the Adjoint Local Solution Marker will take a value between  and .The

Mode Amplitude Cutoff defined in the Stabilized Scheme Settings dialog box defines the lower

The surface shape-sensitivity fields contain the derivatives of the chosen observable with respect to

the position of the bounding walls of the problem.

In the Vectors dialog box, under Vectors of..., you can find the following custom vector fields:

Sensitivity to Body Forces (Cell Values)

This vector field shows how sensitive the observable of interest is to the presence of body forces within

the flow. A body force that locally has a component in the direction of the body-force sensitivity vector

will lead to an increase in the observation of interest.The larger the sensitivity vector, the larger the effect

that a body force can have on the observation of interest.The first-order effect of a body force distribution

per unit volume can be computed as a volume integral of the vector product of the body force distribution

with this field.

Sensitivity to Shape field defined on walls

This vector field shows the postprocessed adjoint solution, independent of any morphing settings, that

defines the sensitivity of the observable of interest to movement of the walls. Deformation of a wall

where this vector is large can be expected to have a significant effect on the observable. In contrast,

deformations of the wall in locations where this vector is small in magnitude, to first order, will have no

effect on the observable.

Optimal Displacement

The optimal displacement field is defined once a design change has been computed using the Design

Tool.This vector field shows the optimal displacement based on the design goals that have been specified

and any prescribed boundary motions. Note that when plotting this vector field, if the Auto Scale option

is deselected, and the vector Scale option is set to , then the vectors as shown display the absolute

displacement that will occur.

Sensitivity to Boundary Velocity

This sensitivity field is defined on boundaries where velocities are specified as an input for the boundary

condition.This includes no-slip, and slip walls.When plotted, this field illustrates where a change to the

boundary velocity can affect the observation of interest.When plotted on a wall, it shows how the im-

position of a nonzero velocity condition on the wall will affect the observation.This can include movement

in the plane of the wall itself.When plotted, for example on a velocity inlet, this field illustrates how

local adjustments to the velocity of the incoming flow affect the observation of interest. Integrating a

potential change to the velocity field, weighted by this sensitivity field over the boundary provides a

first order estimate of the effect of the change on the observation of interest.

Sensitivity to Boundary Mass Flux

This sensitivity field that can be used to visualize the effect of adding or removing fluid via a wall-normal

jet.This can be used, for example, to identify regions on walls where the introduction of suction could

have a significant effect on the observable that has been specified. A plot of the Sensitivity to Boundary

Velocity in general provides a richer view, but sometimes at the expense of the clarity of the visualization.

The computed adjoint solution can provide sensitivity information for individual boundary condition

settings through the Adjoint Reporting dialog box. This dialog box is accessed by clicking Reporting...

in the Design ribbon tab (Adjoint-Based group box).

Design → Adjoint-Based → Reporting...

Figure . : Adjoint Reporting Dialog Box

Boundary condition sensitivity data is retrieved as follows:

Select a single boundary of the problem in the Boundary Choice selection box.

Click Report to see the boundary condition settings and the sensitivity of the observable with respect to

those settings. An example of a report is shown below:

Velocity inlet id

Velocity magnitude = .000000000e+ (m/s),

Sensitivity = .429127866e+ ((n)/(m/s))

In this case, the report shows that for every change of the boundary velocity by  m/s, a change

in the predicted observable (in this case a force) of . N is expected. This prediction is based on

a linear extrapolation.

Click Write... to write the report for the selected boundary to a file.

Tools to modify the boundary and interior mesh of the problem based on the adjoint solution are

provided in the Design Tool dialog box. The Design Tool uses computed adjoint sensitivity data to

find an optimal design change satisfying one or more goals or constraints, and to predict the resulting

changes in observable values. Among the goals that can be specified in the Design Tool are:

minimization, maximization, or targeted changes of single or multiple observable values

prescribed forms of deformation for selected geometry

general constraints on deformations including restrictions on direction of motion, symmetry, and boundary

equality and/or inequality constraints on geometry (fixed walls, bounding boxes, and so on).

The Design Tool is accessed by clicking Design Tool... in the Design ribbon tab (Adjoint-Based group

box).

Design → Adjoint-Based → Design Tool...

Figure . : Design Tool Dialog Box

The general procedure to use the Design Tool is as follows.

.

Select the appropriate Morphing Method for your problem. In general, if you prefer mesh quality

over adherence to the design conditions, you should select Polynomials; otherwise, you should

.

select Direct Interpolation. For details on how they calculate the displacement of the mesh nodes

and their relative merits, see Smoothing and Mesh Morphing (p. ).

.

Select those boundaries that are free to be deformed in the Zones To Be Modified field on the

Design Change tab. Boundaries that are not selected in this box that intersect the control volume

will be constrained not to move. This is useful if there are walls which, for design reasons, must

not move.

Note

If you have a two-sided wall that you want to deform, it is recommended that you select

both the wall and the corresponding wall-shadow.

When using the Direct Interpolation morphing method, you must ensure that none of

the zones involved in a non-conformal mesh interface are selected.

.

Define the region that will be modified in the Region tab. (Defining the Region for the Design

Change (p. ))

.

Define conditions on the deformation region such as number of control points, symmetry, directional

invariance, and boundary continuity. (Defining Region Conditions (p. ))

.

Export the sensitivities from the adjoint solution for each observable of interest. (Exporting Sensitivity

Data (p. ))

.

Import the sensitivity data for each observable that will participate in the design change and specify the

optimization goals for the observables. (Defining Observable Objectives (p. ))

Note

Export and Import of sensitivity data is only required for multi-objective analysis.

.

Define constraining and/or deformation conditions on the design change, such as fixed boundaries,

Note

.

prescribed forms of boundary deformation (through a profile, translation, rotation, scaling, or rigid

body motion), and bounding surfaces / planes. (Defining Conditions for the Deformation (p. ))

.

(optional) Adjust the optimal design calculation numerics if required. (Design Tool Numerics (p. ))

.

Specify the design conditions to be applied (and whether they are strictly enforced), the weights

for the various objectives, and the deformation parameters; then compute the optimal design

change and modify the mesh. (Shape Modification (p. ))

Details of these steps are elaborated in the following sections:

.... Defining the Region for the Design Change

.... Defining Region Conditions

.... Exporting Sensitivity Data

.... Defining Observable Objectives

.... Defining Conditions for the Deformation

.... Design Tool Numerics

.... Shape Modification

Note that if you are setting up the Design Tool in preparation to use the Gradient-Based Optimizer,

you will need to perform most—but not necessarily all—of the previous steps; for details, see Using

the Gradient-Based Optimizer (p. ).

To define the region of space where a design change is to be applied, perform the following steps:

.

Click the Region tab of the Design Tool dialog box.

.

Make a selection from the Region Geometry drop-down menu to specify whether you will define the

space as either a Cartesian or a Cylindrical region type.

.

The Show Bounding Region option is enabled by default, so that you can view the region in the

.

graphics window as it is defined.

.

The simplest way to set up the bounding region is to click the Get Bounds... button. In the Bounding

Region Definition dialog box that opens, you can select the Zones to Be Bounded and click OK to

define a region that encompasses those zones.The following options are enabled in the Bounding

Region Definition dialog box by default:

The Comfortable Region option specifies that the region is slightly larger than selected zones.You

can disable this option if you want the region to exactly adhere to the extents of the selected zones.

For the Cylindrical region type, the Automatic Coordinate option defines the origin and axis of the

region to match those defined for the selected zones (if possible).This is helpful when a selected

zone has been defined as rotationally periodic, or is adjacent to a cell zone that has the Frame Motion

option enabled as part of a rotating reference frame problem.

If necessary, you can then click the Larger Region and/or Smaller Region buttons to adjust the

size of the region.

.

If you need more precise control over the definition of the region, you can enter values directly for the

settings.

For the Cartesian region type, you can specify the X Min, X Max, Y Min, and Y Max (and Z Min

and Z Max in 3D) fields.

For the Cylindrical region type, you can specify the angular, radial, and (for 3D) axial coordinate

ranges; this will require you to define a Coordinate System, and then enter the values of the

Region Extent relative to that system. The fields you will define are illustrated in Figure . : A

Cylindrical Region (p. ).

Figure . : A Cylindrical Region

Note the following for Cylindrical regions:

For 2D cases, the axis is defined implicitly as the Z-axis (as determined by the right-hand rule,

where in a front view the X-axis is horizontal and the Y-axis is vertical).

For the angular range (defined by Theta Min and Theta Max), the positive direction is determined

by the right-hand rule about the axis, and the total range must not exceed  degrees.

For 3D cases, the axis and radial direction must not be co-linear.

Radial symmetry is not possible.

After you have entered the settings, click Update Region to set the values and update the display.

Note

Symmetry conditions affect the location and size of the region:

If you plan to enable the Symmetry of Motion options in the Region Conditions tab (as

described in Defining Region Conditions (p. )), the region should be positioned with

forethought given to the effect on the various boundary zones in the region.

If you have a boundary zone of type symmetry in the region, it is recommended that it

either is located on a planar boundary of the region, or is centered within the region in a

manner that is consistent with the Symmetry of Motion option.

To define the region conditions, perform the following steps. Note that all of the settings described

in this section (except for the Motion Enabled options) are either unnecessary or not supported

when using the direct interpolation method for morphing, and are thus not available for editing.

.

Click the Region Conditions tab in the Design Tool dialog box.

.

.

.

Specify the control points and motion conditions for each coordinate direction.

a.

Select the number of control Points.

The control points are distributed uniformly within each coordinate range (in the X-, Y-, and

Z- directions for a Cartesian region, and the Theta, Radial, and Axial directions for a cylindrical

region). The spacing between the control points defines the characteristic spatial scale for

the deformation operation. The larger the number of control points, the smaller the spacing

and hence, the smaller the spatial scale on which changes can be made. to  control

points for each coordinate direction is typical.

Note that the control points are displayed in red (and updated when you click Apply) along

representative directions of the region in the graphics window, in order to allow you to

visually determine if the number you have specified is appropriate.

b.

If you want to prevent deformation in the given coordinate direction, disable Motion Enabled.

c.

If you want the motion along a coordinate direction to be uniform in one or more directions, enable

the appropriate option (for example, Invariant in X).

d.

You can ensure that the deformation is symmetrical relative to the different coordinate directions

by enabling options in the Symmetry of Motion group box. Symmetry can be imposed in as many

directions as desired (though radial symmetry for a cylindrical region is not possible).The symmetry

planes will be displayed in the graphics window when you click Apply; you should ensure they

reflect your intent for the design change, modifying the extents of the deformation region as ne-

cessary.

.

The Region Boundary Continuity settings control the order of continuity of the deformation process

at the boundaries of the deformation region.This is of particular relevance when the boundary of the

deformation region intersects a wall that will be deformed.The Continuity Order controls the

smoothness of the transition from the undeformed wall lying outside the deformation region to the

deformed wall within. A value of  ensures first-order continuity at the transition, that is, a continuous

first derivative of the deformation operation. A value of  ensures second-order continuity, and so on.

By default, the continuity Definition is Uniform and is enforced at all deformation region

boundaries. Alternatively, you can choose By Boundary to use different continuity conditions

at each boundary. For each boundary (X-Min, X-Max, and so on) you can specify what order

continuity to enforce for each motion direction. You can also specify In-Plane Motion Only on

that boundary; note that this option may be useful if a deformation region boundary coincides

with a boundary zone that is of type symmetry.

The continuity settings will not affect the transition between fixed and movable boundaries

within the deformation region, only mesh nodes in the transition zone from inside to outside

the deformation region.

.

.

In order to perform multi-objective optimization, you need to export the sensitivity data for each

observable/flow-condition combination that will take part in the optimization.

.

Define the observables of interest as described in Defining Observables (p. ).

.

For each observable solve for and export the sensitivity data.

a.

Solve the adjoint as described in Solving the Adjoint (p. ).

b.

Click the Manage Data... button in the Objectives tab of the Design Tool dialog box, and

then click the Export... button in the Manage Sensitivity Data dialog box that opens.

The exported file contains the sensitivities of the observable for the mesh nodes within the specified

deformation region. The deformation regions for the various observables can, in principle, be different.

However, it is advisable that there is as much overlap as possible for observables that will be used

together in a multi-objective design process.

The Design Tool computes the optimal mesh deformation to satisfy multiple simultaneous design

goals. Among these can be goals for multiple observables, possibly at multiple flow conditions. Once

you have obtained the adjoint solutions and displacement sensitivities for the various observables of

interest, you can import the data and specify the design objectives for each.

.

Click the Objectives tab in the Design Tool dialog box.

.

To import previously saved sensitivity data, click Manage Data.... Then click the Import... button

in the Manage Sensitivity Data dialog box that opens to load previously saved sensitivity files.

Close the Manage Sensitivity Data dialog box when done.

.

If you want to include computed sensitivity data in the current session that you have not exported yet

enable Include Current Data.

.

For each observable objective you can specify the following.

Objective

determines how Fluent will attempt to change the value of the observable through the design

change.You can choose to increase or decrease the value of the observable optimally, or you can

specify a target change in value.You can also select None in which case the observable will not be

considered in computing the optimal design change, but the predicted change in observable value

will still be reported.

Target/Reference Change

When the chosen Objective is Target Change in Value, this field corresponds to the desired change

in the value.When the chosen Objective is Maximize or Minimize, the magnitude of this field is

a reference weighting for the observable.This can be used to normalize the objectives in cases

where you have multiple observables of vastly differing magnitudes, thereby allowing the values

entered for Weight in the Design Change tab to all be of similar scale.You can check As Percentage

to specify the Target/Reference Change as a percentage of the value of the observable.

Note

You must click Apply for each objective you define before moving on to the next

one.

In the Design Conditions tab, you can specify conditions on the mesh morphing such as fixing portions

one.

of wall surfaces, prescribing the deformation of surfaces, or setting up bounding planes / surfaces.

To create a condition, click Create..., select the type of condition in the Create New Condition dialog

box (you can choose between fixed-walls, bounded-by-plane, bounded-by-surfaces, prescribed-

profile, rotation, translation, scaling, and rigid-body), and provide a unique Name. You can then

define the condition by selecting it in the Defined Conditions list on the left, defining the settings

(as described in the steps that follow), and clicking Apply. If necessary, you can Rename a selected

condition using the Rename Constraint dialog box that opens. Once created, the design conditions

can be individually included or excluded from the design change in the Design Change tab.

At any time you can click the Display button so you can view the surfaces of the selected design

condition in the graphics window. The type of design condition is indicated by the color of the surface.

Clicking the Display Options... button opens the Design Condition Display Options dialog box,

where you can set the following additional options:

The Auto-Display option specifies that the graphics window automatically updates whenever a design

condition is created or selected, as well as when the Apply button is clicked.

The Schematic option specifies that settings for the design conditions are also displayed in the graphics

window, including origins, axes, planes, and normals.

When using the Polynomials morphing method, design conditions are not applied to every node, but

instead to a subset of nodes distributed throughout the selected surfaces; this is to avoid overly constraining

the zone.The Constrained Nodes option in the Design Condition Display Options dialog box allows

you to highlight the nodes of this subset.This can help you determine if the number of control Points

defined in the Region Conditions tab / size of the region is appropriate for the surfaces involved in your

design conditions; if the density of constrained nodes is not sufficient, you should either increase the

number of controls points or reduce the size of your region. Note that the constrained nodes are only

relevant for surfaces that are not selected in Figure . :The Strict Conditions Dialog Box (p. ).

Figure . : The Design Condition Display Options Dialog Box

Note that the adjoint solver's prediction range is reduced when you include design conditions—es-

pecially prescribed-profile, rotation, translation, scaling, and/or rigid-body conditions—so you

should attempt smaller deformations (for example, when setting the Target/Reference Change in

the Objectives tab).

Important

A given surface cannot have multiple conditions of type prescribed-profile, rotation,

translation, scaling, or rigid-body.

Fixed Walls

The fixed-walls constraint can be applied to clip-surfaces of walls in the deformation region. This

offers a fine-grained control over parts of the geometry that should not move. Whereas deselecting

a zone in the Zones To Be Modified list on the Design Change tab will fix an entire wall zone, se-

lecting a clip-surface from in the Fixed Walls Condition list will fix only the portion of the wall that

forms the clip-surface.

Any clip surfaces you have defined will appear in the Clip Surfaces list. You can assign clip surfaces

to a fixed walls constraint by selecting them in the list and clicking Apply.

Bounding Planes

The bounded-by-plane condition allows you to define one or more bounding planes that constrain

the geometry deformation in such a way that the geometry cannot cross the given planes, thereby

respecting packaging or form-factor constraints. The bounding plane is characterized by a vector

normal to the plane and a distance measured from the global coordinate system origin to the plane,

along the normal direction. The motion of the selected wall surface(s) will be constrained such that

all points on the surface(s) lie on the side of the bounding plane that is opposite to the normal direc-

tion.

Figure . : Specifying a Bounding Plane for Design Changes

Origin

d<

wall surface

bounding plane

n

r

Origin

d>

n

r

In Figure . : Specifying a Bounding Plane for Design Changes (p. ) the bounding plane normal

vector is denoted by  and the distance is denoted by . is the position vector of a point on the

wall surface subject to the bounded-by-plane condition. Note that a positive value for the distance

yields a bounding plane that is oriented with its normal pointing away from the origin, while a neg-

ative value for the distance yields a bounding plane oriented with its normal direction pointing towards

the origin. The constraint equation can be expressed as:

.

Select the surfaces (or clip-surfaces) that are subject to the bounding plane condition in the Bounded

.

Enter the components of the bounding plane normal direction.

.

Enter the distance of the plane from the origin (along the normal direction).

.

Bounding Surfaces

The bounded-by-surfaces condition allows you to import one or more bounding surfaces that con-

strain the geometry deformation in such a way that the geometry cannot cross the nearest facet of

the bounding surfaces, thereby respecting packaging or form-factor constraints; alternatively, you

can prescribe that the geometry deforms to conform to the bounding surfaces. The bounding surfaces

can be read from an .stl, .msh, or .cas file. The deformation of the selected bounded surfaces

will be constrained such that all points on the surfaces lie on the sides of the bounding surfaces that

have a positive orientation.

.

Select the surfaces (or clip-surfaces) that are subject to the bounded-by-surface condition in the Bounded

.

Use the Read... button to import a .stl, .msh, or .cas file that contains the appropriate bounding

surface(s). Note that the file you read must have the same dimensionality (2D or 3D) as the working

case file.

.

Select the Imported Surfaces that will constrain the bounded surfaces.

.

To visually confirm that the selected Bounded Surfaces and Imported Surfaces are appropriate, click

.

the Display button.The imported surfaces will be colored green by default.

Note

When examining the surfaces, it may be helpful to revise display properties of partic-

ular surfaces (for example, the color, the level of transparency, and the visibility of the

mesh edges or faces). This can be done using the Scene Description dialog box, as

described in Advanced Scene Composition (p. ). Note that you can even revise the

display properties of the imported surfaces, the names of which will be displayed with

the prefix bounding-.

.

When constraining the Bounded Surfaces, you should ensure that they are constrained on the

correct side of the Imported Surfaces (that is, the side that has a positive orientation) by clicking

the Orientation... button. The selected Imported Surfaces will be displayed, with their orientation

indicated by arrows. In the dialog box that opens (Figure . : The Bounding Orientation Dialog

Box (p. )), you can select individual Bounding Surfaces and Reverse their orientation as ne-

cessary; you can also increase the Skip value to display fewer orientation arrows, for cases where

the arrow density obscures the orientation. Note that the orientation you define for a particular

bounding surface will be used globally for all bounded-by-surfaces conditions.

Figure . : The Bounding Orientation Dialog Box

When reviewing the orientation of a bounding surface, you should verify that the facets have a

uniform orientation, that is, all of the arrows are on the same side of the surface. Bounding surfaces

with facets that have a mixed orientation can affect the convergence and/or accuracy of the

.

.

To prescribe that the Bounded Surfaces deforms so as to conform to the Imported Surfaces,

enable the Fit to the imported surfaces? option. This is only recommended when the bounded

and imported surfaces are very similar in shape and separated by a small distance (on the order

of the local cell dimensions).

.

Click Apply in the Design Conditions tab of the Design Tool dialog box to save your settings.

.

If at any point you would like to delete any of the Imported Surfaces, select them and click the

Delete button below the list. You can also delete them using the Surface Meshes Dialog

Box (p. ).

Note

When using the bounded-by-surfaces condition, it is recommended that you apply pre-

conditioning on the advancement of the process for updating the freeform displacements

(by changing the Preconditioning field to a positive value in the Numerics tab of the

Design Tool dialog box, as described in Design Tool Numerics (p. )), in order to encour-

age the stability of the solution. A value on the order of  or  is recommended.

Prescribed Profiles

You can use the prescribed-profile condition to assign a motion profile to a wall zone or zones using

a DEFINE_GRID_MOTION UDF.

.

Select the wall zones to undergo displacement in the Wall Zones list.

.

Compile your DEFINE_GRID_MOTION UDF in Fluent. (Refer to DEFINE_GRID_MOTION in the Fluent

Customization Manual).

.

Select your UDF in the Deformation profile drop-down list.

.

Define the Scale Factor to be applied to the deformation profile. You have the following options:

Enter a set value.

.

.

Use the drop-down menu to define the scale factor through an expression or input parameter (for

example, as part of a parametric study managed by Workbench); for details, see Directly Applied Ex-

pressions (p. ) or Creating a New Parameter (p. ), respectively.

Disable the Prescribed option so that the scale factor is a free parameter.This can be helpful when

you are trying to optimize a design, because the Design Tool will determine a scale factor that satisfies

your goals, and so no input is required from you.The value will be determined when you calculate

the design change, and will be printed in the console; the printed value can be useful if you would

like to recreate the design change in another software program (rather than exporting it as an .stl

file).

.

Rotation

The rotation condition allows you to specify that surfaces undergo rotation.

.

Select the surfaces (or clip-surfaces) you want to rotate in the Surfaces list.

.

Define the rotation Angle. You have the following options:

Enter a set value in degrees.

Use the drop-down menu to define the angle through an expression or input parameter (for example,

as part of a parametric study managed by Workbench); for details, see Directly Applied Expres-

sions (p. ) or Creating a New Parameter (p. ), respectively.

Disable the Prescribed option so that the rotation is a free parameter.This can be helpful when you

are trying to optimize a design, because the Design Tool will determine an angle that satisfies your

goals, and so no input is required from you.The value will be determined when you calculate the

design change, and will be printed in the console; the printed value can be useful if you would like

to recreate the design change in another software program (rather than exporting it as an .stl file).

.

Define the Origin about which you want the surfaces to rotate. Note that you can click the Get

Center button to set the origin fields to the coordinates of the center of the selected surfaces.

.

For 3D cases, define the Axis of rotation. For 2D cases, this is automatically defined as the positive Z

axis.

.

Translation

The translation condition allows you to specify that surfaces undergo translation.

.

Select the surfaces (or clip-surfaces) you want to translate in the Surfaces list.

.

Define the Displacement for each coordinate axis. For each field you have the following options:

Use the drop-down menu to define the displacement through an expression or input parameter (for

Disable the Prescribed option so that the translation is a free parameter.This can be helpful when

you are trying to optimize a design, because the Design Tool will determine a displacement that

satisfies your goals, and so no input is required from you.The value will be determined when you

calculate the design change, and will be printed in the console; the printed value can be useful if you

would like to recreate the design change in another software program (rather than exporting it as

an .stl file).

.

Scaling

The scaling condition allows you to specify that surfaces are scaled along one or more axes.

.

Select the surfaces (or clip-surfaces) you want to scale in the Surfaces list.

.

Select the scaling Type and define the associated settings:

Radial

This type scales the surfaces radially about the Origin, using a single scaling Factor along

each of the coordinate axes. The size of the surfaces will change, though not the shape.

In-Plane

This type is available for 3D cases, and scales the surfaces about the Origin using a single

scaling Factor along the two axes of a plane (as defined by the Normal Direction).

Axial

This type scales the surfaces about the Origin using a scaling Factor along a single Axis.

General

This type scales the surfaces about the Origin using a separate scaling Factor for each of the

defined axes. For 2D cases, you define one Axis, and the second axis is automatically defined

as being perpendicular; for 3D cases, you define Axis  and Axis  (which should not be par-

allel), and the third axis is defined automatically as the cross product. Note that the surfaces

will be scaled along each axis sequentially, so the order will be relevant for non-orthogonal

axes.

For all types, the scaling Factor must be positive. A value of  results in no change, while a value

greater or less than  results in stretching or shrinking, respectively. You have the following op-

tions:

tions:

Use the drop-down menu to define the factor through an expression or input parameter (for example,

Disable the Prescribed option so that the factor is a free parameter.This can be helpful when you

are trying to optimize a design, because the Design Tool will determine a factor that satisfies your

When you are defining the Origin for any of the types, note that you can click the Get Center

button to set the origin fields to the coordinates of the center of the selected surfaces.

.

Rigid Body Deformation

The rigid-body condition allows you to specify that surfaces undergo rigid body motion, in which

the rotations and translations are free parameters. The Design Tool will determine rotations and

translations that satisfy your goals when you calculate the design change, and will print them in the

console. The printed values can be useful if you would like to recreate the design change in another

software program (rather than exporting it as an .stl file); note that you must apply the deformations

in the same order as they are printed to obtain the same results.

.

Select the surfaces (or clip-surfaces) you want to undergo rigid body motion in the Surfaces list.

.

.

.

Smoothness

As described in Smoothing and Mesh Morphing (p. ), there are two morphing methods available

for the adjoint solver. The following describes how smoothing is performed in each:

polynomials-based approach

In this approach, the mesh morphing is controlled by the summation of two smoothing bases: the

Bernstein polynomial basis which control the large scale smooth deformation and the B-spline basis

which controls fine-scale deformation. The choice of smoothness determines the relative weighting

of these bases and therefore the spatial scale of the design change. A large value of smoothness

biases the design change to one in which optimal displacements vary in space in a manner domin-

ated by the Bernstein polynomial basis. That is, they have a high degree of smoothness. A smaller

value of smoothness leads to a recommended design change with smaller spatial scales.

The ability to vary the smoothness parameter is particularly important when prescribed forms of

deformation are applied. Deformation at smaller spatial scales relieves the stiffness that would

otherwise cause numerical challenges as well as lead to poor quality of the computed design and

mesh.

direct interpolation method

In this method, the surface mesh is smoothed using a Laplacian smoothing approach. Unlike the

polynomials-based approach, the smoothness input does not effect the convergence of the design

conditions, but it has a strong impact of the smoothness of the displacement on the surfaces un-

dergoing free deformation. This is an important parameter in the direct interpolation method.

By default, Fluent will automatically define the smoothness. You can disable Auto-Select Smoothness

in the Numerics tab, and then a Smoothness input will be available in the Design Change tab. The

default value of  for Smoothness is suitable for a variety of cases; a reasonable range for this field

is between - and .

Calculation Numerics

Note

If no Design Conditions are imposed, and if there are no walls that are treated as fixed

which intersect the region being modified, the numerical settings described below are not

used.

In many cases, no adjustment of the detailed numerics will be required for the Design Tool to compute

an optimal solution. However, if the problem under investigation involves many Design Conditions

and/or large displacements, the settings may need to be adjusted. Note that all of these fields (except

for Max. Iterations in the Freeform Motions group box) are not needed when using the direct inter-

polation method for morphing, and are thus not available for editing.

Prescribed Motions

The following settings apply to cases that involve the prescribed-profile, rotation, scaling, translation,

and/or rigid-body design conditions.

Max. Iterations

The maximum number of inner iterations that will be performed in an effort to compute displacements

from prescribed changes.

Constraint Relaxation

The under-relaxation factor that is applied to the field to converge the prescribed displacements.

This takes a value between  and .

Preconditioning

A value of  yields the most aggressive advancement, while a larger value encourages more stable,

albeit slower, advancement of the process for updating the prescribed displacements. A value of

order  is typical in the event that preconditioning needs to be applied.

Freeform Motions

The maximum number of inner iterations that will be performed in an effort to compute freeform

displacements that satisfy the applied Design Conditions.

The under-relaxation factor that is applied to the field to converge the constrained freeform displace-

ments.This takes a value between  and .

A value of  means that no preconditioning is applied, while a larger value encourages more stable,

albeit slower, advancement of the process for updating the freeform displacements. A value of order

is typical in the event that preconditioning needs to be applied.

Parameter Relaxation

For cases that include a rigid-body condition and/or a design condition with a free parameter

(for example, the rotation condition with Prescribed option disabled for the Angle), there

are additional parameters that are implicit in the calculation. The values of these parameters

are computed as part of the solution process. The value of the parameter relaxation defines

the rate at which these parameters are corrected as the calculation progresses. This takes a

value between  and .

Tolerances

Constraints

The tolerance for convergence of the residuals associated with the design conditions themselves,

or fixed zone conditions.

The tolerance for convergence of the parameters associated with the design conditions.

Using a value of  for Constraint Relaxation and a value of  for Preconditiong yields the most

aggressive behavior. This can result in the fewest number of iterations to converge a constrained

problem, at the expense of some added numerical effort and memory in preparing the preconditioning.

For 2D and small 3D problems the added cost in time and memory is typically small. For larger

problems involving multiple constraints a non-zero Preconditioning and Constraint Relaxation less

than  may be preferable. The execution time to set up the preconditioning will be less, as will the

memory usage. Calculation stability can also be improved. The number of iterations required to con-

verge the problem will increase. However, this can prove to be an effective strategy that results in

an overall shorter time needed to compute the design change.

The procedure for computing the optimal design change and deforming the mesh is as follows:

.

Click the Design Change tab.

.

Select those boundaries that are free to be partially constrained or deformed in the Zones To

Be Modified field. Boundaries that are not selected in this box that intersect the control volume

will be constrained not to move. This is useful if there are walls that, for design reasons, must

remain fixed and not move.

Note

Note

.

Select the constraining and/or deformation conditions (Defining Conditions for the Deforma-

tion (p. )) to be applied to the design change in the list of Applied Conditions. Note that a

given surface cannot have multiple conditions of type prescribed-profile, rotation, translation,

scaling, or rigid-body.

You can click the Display button under the Applied Conditions list, in order to display the applied

conditions in the graphics window, each type in a unique color. Note that this includes the

conditions selected in the list, as well as the fixed conditions applied to zones that are not selected

in the Zones To Be Modified list. This makes it easy to review your setup, and identify any

overlapping conditions (recognizable by their two-tone cells).

.

When using the Polynomials morphing method, by default the condition or conditions specified

for a given zone (including the selected Applied Conditions, as well as the fixed condition applied

to the unselected Zones To Be Modified) are not applied to every node, but instead to a subset

of nodes distributed throughout the zone; this is to avoid overly constraining the zone. Con-

sequently, some nodes will not strictly adhere to the condition, even if you have defined the

constraint tolerance to be small or the residuals are small. To specify that all nodes of the zone

strictly obey the condition, click the Strict Conditions... button under the Applied Conditions

selection list and use the dialog box that opens (Figure . : The Strict Conditions Dialog

Box (p. )).

Figure . : The Strict Conditions Dialog Box

Select the conditions for which you want strict enforcement and click OK. For unselected condi-

tions, only the default subset of nodes will strictly obey the condition. Note that when you apply

strict enforcement to a case in which the Objective is Target Change in Value (as described in

Defining Observable Objectives (p. )), the desired change in the value may not be achieved.

Note

Strict enforcement is a direct modification of the surface mesh nodes to satisfy the

design condition, and no modification is applied on the interior mesh. Consequently,

when the boundary node modification is large, it may deteriorate the mesh or even

cause negative volumes. Therefore you should use this condition carefully: the design

condition should reach a good convergence and there should be enough control

points.

When you click the Modify button (as described in a later step), the maximum offset for each

condition (that is, the maximum distance a node has deviated from the prescribed condition)

will be printed to the console.

.

For each observable, specify its Weight in the optimization calculation.The weights are applied to the

Target/Reference Change you specified in the Objectives tab.That is, if you have two observables

that are each given a Weight equal to , Fluent will attempt to find an optimal design change that alters

the observable values in proportion to their respective values for Target/Reference Change.

Note

Weights are only required if there are two or more objectives that do not have explicit

target changes specified.

.

Specify the deformation parameters.

a.

When using the Polynomials morphing method, choose a Freeform Scaling Scheme and

specify the Freeform Scaling Factor. This setting controls how the overall scaling factor for

the design change magnitude is interpreted.

Control-Point Spacing

The magnitude of the freeform deformation will be based on the control-point spacing.

That is, a Freeform Scale Factor of . leads a to maximum control point movement on

the order of one sub-cell of the control volume.The sub-cell size is determined by a uniform

sub-division of the morphed region based on the number of control points specified

(Defining Region Conditions (p. )). A value of . is a reasonable default to preserve

mesh quality during the morphing process.

Objective Reference Change

The magnitude of the freeform deformation will be based on the Target/Reference

Change value in the Objectives tab.That is, for a single observable optimization with

Freeform Scale Factor of ., the design change computed will yield an expected change

in the observable equal to the Target/Reference Change for the observable.

b.

If you have disabled Auto-Select Smoothness in the Numerics tab, you can also specify a value

for Smoothness of the deformed geometry. A lower value will allow locally sharper changes in

the geometry, potentially at the expense of manufacturability. For details about this setting, see

Design Tool Numerics (p. ).

c.

c.

If you used an input parameter as part of the setup of a deformation condition in the Design

Conditions tab, the initial value will be displayed and is available for modification.

.

Click the Check button to verify that your constraining and/or deformation conditions are set up in

such a way as to produce good results. A report will be printed in the console listing conflicts between

multiple constraints / deformations applied on a single node (including the Design Conditions and

the continuity constraint applied along the boundary of the morphing region).The conflicts are categor-

ized as being either of type Fatal (which indicates the solution is unlikely to converge or be desirable)

or Possible (which may be allowable, depending on the details of the applied conditions).

.

Click Calculate Design Change to compute the optimal design change.The Expected change for each

observable will be reported in the Design Tool dialog box.

.

(optional) You can export the expected changes or displacements by clicking the Export... button

and clicking the following buttons in the Design Export dialog box that opens:

Click Export Expected Change... to write to file the adjustment in the observable that is expected

due to the change defined by the current settings.

Click Export Displacements... to write to file the optimal surface displacement field (overwriting

any pre-existing file of the same name). An example of the format of the text file that is written (for

three-dimensions) is as follows:

Line : n

Lines  to n+: x y z dx dy dz

Figure . : The Design Export Dialog Box

Line : n

. The planned change to the geometry can be displayed in the graphics window by clicking the

Preview... button and then using the Preview Morphing dialog box that opens to display the

surfaces of interest. Note that you can use the buttons to easily select all the Outline boundaries

and/or the Interior surfaces, and you can increase the Scale to accentuate the morphing preview

or exported .stl. When you click the Display button, the selected surfaces are displayed unde-

formed in white and deformed in green.

Figure . : The Preview Morphing Dialog Box

Note that for 3D cases you can also use the Export STL... button to export the previewed mesh

as an .stl file. This is useful for large cases, as it means you do not have to actually morph the

mesh in order to have the previewed geometry available for use in other software packages.

. Click the Modify button in the Mesh group box to deform the boundary and interior mesh with

the optimal design change. You should then examine the modified shape and mesh to determine

if the results are satisfactory, using the usual commands for viewing the mesh in ANSYS Fluent.

When using the Direct Interpolation morphing method, it is recommended that you check the

resulting mesh quality and verify that no boundary zones cross / penetrate themselves or other

boundary zones. If you determine that the change is unsatisfactory, you can click Revert to undo

the mesh changes.

After the mesh has been modified according to the control settings, the original flow calculation can

be restarted and converged with the modified geometry. Upon successful convergence, the observable

value should now have changed by an amount similar to that reported when the Export Expected

Change... button was clicked prior to deforming the geometry.

For 3D cases, you have the option of exporting the surfaces from your modified geometry as an .stl

file, for use in other software packages. Click the Export... button near the bottom of the Design

Change tab and then click the Export STL... button in the Export dialog box that opens. Finally, select

the Surfaces of interest in the dialog box that opens (Figure . : The Export STL Dialog Box (p. ))

and Export... them.

Figure . : The Export STL Dialog Box

The adjoint solver provides an Gradient-Based Optimizer that can automatically create a series of it-

erations of a design, so that the mesh gradually deforms to an optimal shape in order to meet multiple

objectives at multiple operating conditions. To prepare to use the Gradient-Based Optimizer, you

will perform most of the usual steps outlined in Using the Adjoint Solver (p. ) (including the setup

of the Design Tool), with the following exceptions:

It is not necessary to start with a converged flow solution; simply initializing the case file is sufficient.

It is not necessary to select a single observable in the Adjoint Observables dialog box, as you will be able

to select multiple observables in a separate dialog box.

It is not necessary to initialize the adjoint solution and iterate to convergence using the Run Adjoint Cal-

culation dialog box, as these actions will be performed in the Gradient-Based Optimizer dialog box.

When setting up the Design Tool:

– It is not necessary to export / import sensitivity data, as this will be handled automatically during optim-

ization.

– It is not necessary to specify the objectives for the observables in the Objectives tab of the Design Tool

dialog box, as this will be done in the Gradient-Based Optimizer dialog box.

– In the Design Change tab of the Design Tool dialog box, it is not necessary to take any action in the

Workflow, Mesh, and Results group boxes.

Note that while the above steps are not necessary, you may yet want to perform them in order to

verify that your settings are properly defined (for example, to ensure your design conditions are not

conflicting) prior to using the optimizer.

To start, you must define the settings for the flow solution and initialize it; if you want to optimize the

design for multiple operating conditions, as part of this step you should create input parameters for

the cell zone and boundary condition settings you would like to vary. Next, you must define the adjoint

observables, methods, solver controls, monitors, and Design Tool, noting the exceptions listed previ-

ously. Then you can open the Gradient-Based Optimizer dialog box by clicking Gradient-Based

Optimizer... in the Design ribbon tab (Adjoint-Based group box).

Design → Adjoint-Based → Gradient-Based Optimizer...

Figure . : Gradient-Based Optimizer Dialog Box

The general procedure to use the Gradient-Based Optimizer is as follows:

.

Click the Observables... button to open the Adjoint Optimizer Observables dialog box, where you

can select all of the relevant observables for your optimization problem and click OK.

Figure . : Adjoint Optimizer Observables Dialog Box

.

Click the Conditions... button to open the Adjoint Optimizer Conditions dialog box.

Figure . : Adjoint Optimizer Conditions Dialog Box

Define the following:

Number of Operating Conditions

This defines the number of possible operating conditions. Each operating condition is a set of simu-

lation properties for which a flow solution will be calculated. As you increase this number, more rows

will be added to the group box below, each with a unique No..The Active? option must be enabled

to calculate the flow for that operating condition.

Number of Input Parameters

This defines the number of input parameters you would like to define for each operating condition.

As you increase this number, more columns will be added to the group box below.You can select

an input parameter from one of the top drop-down lists, and then define its value for each operating

condition in the number-entry boxes below it.

When you have defined all the operating conditions, click Apply, and close the Adjoint Optimizer

Conditions dialog box.

.

Fill out the following columns for the table in the Objectives group box. Each row represents a unique

.

combination of the active operating conditions and the selected observables defined in the previous

steps.

Goal

This determines how Fluent will attempt to change the value of the observable through the design

change.You can specify a Target change in value; otherwise you can select None, in which case the

observable will not be considered in computing the optimal design change, and the predicted change

in observable value will not be reported.

Value

When the Goal is a Target change in the observable, this field corresponds to the desired change

in the value.

Percentage?

Enabling this option specifies that the Value is a percentage of the value of the observable.

A target change of –% is typically a good starting point, depending on the problem.

.

The Adaptive Value option is enabled by default, and is generally recommended.When using this option,

Fluent automatically detects when a design iteration produces non-optimal results (compared to previous

flow solutions), and reattempts the design using Objectives settings that are less aggressive.The process

is as follows: the solution calculated for the initial design is considered optimal and written to disk; then

the following two steps are repeated.

. The design is revised based on the current Objectives settings.

. The flow solution is calculated, and the results are compared to the optimal design solution:

If the values of all of the observables for all of the operating conditions improve or remain the

same, the revised design solution is deemed the new optimal (and the files are overwritten), and

the process returns to step .

If the value of one or more of the observables for any of the operating conditions worsens, the

optimal design solution is restored, the Objectives settings are revised such that every Value is

reduced by % going forward, a new design is generated, and the process returns to step .

When using the Adaptive Value option, note the following:

The naming convention for the optimal design solution files is provided in a later step that describes

how to set up autosaving.

You must ensure that you have sufficient disk space for the optimal design solution files.

You must not remove or rename the optimal design solution files during optimization.

You must ensure that the optimal design solution files are in the correct folder if you stop the optim-

ization and then continue it.

If a problem occurs during optimization, you can either:

– initialize the optimizer again: the current design solution files will be saved as the optimal if optim-

ization continues, and the Curr. Design Iteration will be reset to  and the optimization history in

the monitor plot will be lost.

– reset it: the current design solution files will be saved as the optimal if optimization continues, but

the Curr. Design Iteration will not be reset to  and the optimization history in the monitor plot

will not be lost.

If you stop the optimizer, modify some settings, and then continue the calculation, note that your

changed settings may be overwritten if the optimal design solution is restored during the first iteration.

.

The Optimizer Settings group box allows you to view / set the following:

Curr. Design Iteration

.

This displays the current design iteration.

No. of Design Iterations

This specifies the maximum number of design iterations that the optimizer will perform. A value in

the range of – is typically appropriate, depending on the problem and settings.

Convergence Criteria

This defines the criteria by which the design is considered converged. For every observable at every

operating condition, the following are calculated during various points in the design iteration:

the expected change / initial value (when the design change is calculated)

the actual change / initial value (when the flow solution is calculated)

When either of the above are less than your specified Convergence Criteria for all observables

at all operating conditions, the optimizer will stop iterating.

No. of Flow Iterations

This specifies the maximum number of iterations performed during the calculation of the flow solution.

A starting value of  is typically appropriate, depending on the problem and settings.

No. of Adjoint Iterations

This specifies the maximum number of iterations performed during the adjoint calculation. A starting

value of  is typically appropriate, depending on the problem and settings.

.

Specify the settings in the Mesh Quality group box.

By default, the cell volume and orthogonal quality (as defined in Mesh Quality (p. )) is computed

at the start of every design iteration, before the flow solution is calculated; if the mesh violates

your specified Min. Cell Volume and/or Min. Orthogonal Quality, the optimizer stops. Such a

check is also performed immediately after each design change is calculated; if this check fails,

Fluent reattempts the design using Objectives settings that are less aggressive, in the same

manner as described previously for the Adapted Value option (regardless of whether that option

is enabled). This helps to ensure that your solution accuracy is not compromised by poor quality

meshes. When the direct interpolation method is used, the mesh quality may deteriorate quickly

at local regions, therefore the value will be reduced quickly. You may continue the optimization

by readjusting the value, accordingly. When setting these minimums, you can click the Print

Current Status button and enter values that are sufficiently lower then those printed in the

console, so as not to reject a majority of the meshes generated during the optimization process.

Note that it is recommended that you set the Min. Orthogonal Quality to a value greater than

, in order to avoid left-handed faces.

The Improve Mesh Quality After Morphing option is enabled by default. This attempts to repair

the mesh at the end of the design iteration (after the mesh has morphed) by applying the following

text command  times: mesh/repair-improve/improve-quality. Note that this text

command may deteriorate the mesh in certain circumstances.

.

You can set up a monitor of the optimization history by clicking the Monitor.... button in the Calculation

Activities group box.

Figure . : Adjoint Optimization History Monitor Dialog Box

The Adjoint Optimization History Monitor dialog box has the following controls:

Plot During the Optimization

This option specifies whether plotting is performed for each design iteration.

Observable Values

This option enables the plotting of observable values from the flow calculation.The data is represented

by solid lines.

Expected Observable Values

This option enables the plotting of expected observable values for the next design iteration. It is

calculated by taking the current observable value and adding the expected change due to the mesh

morphing in the current design iteration.The data is represented by dashed lines. If dashed and

solid lines of the same color do not match well, that is a sign that the sensitivity is not accurate for

that observable, and so you may need revise your setup (improve the convergence of the flow and/or

adjoint solvers, reduce optimization values, and so on).

Plot All Optimization IDs

This option enables the plotting of data for all optimization IDs, that is, all of the rows of the table

in the Objectives group box; otherwise, only a single optimization ID will be plotted.

Optimization ID to be Plotted

This field specifies the individual optimization ID to be plotted, and is only available when the Plot

All Optimization IDs option is disabled.The number you enter corresponds to the ID in the Object-

ives group box.

Window

This field sets the ID of the graphics window in which the plot is displayed.

.

You can set up the automatic saving of files during optimization by clicking the Autosave.... button in

Window

.

the Calculation Activities group box. Note that the resulting case and data files will use the Hierarchical

Data Format (HDF) if without any post-fix, such as .cas, .dat, .cas.gz, etc. All of the files will be

saved after the adjoint design calculation but before the morphing of the mesh.

Figure . : Adjoint Optimizer Autosave Dialog Box

The Adjoint Optimizer Autosave dialog box has the following controls:

File Name

This field specifies the root name for the files that are saved. It is suggested that you do not include

an extension for the file name. If you include a folder, you must make sure that it is accessible.

Save Case and Data Files (Every Design Iteration)

This group box allows you to specify settings for the autosaving of case and data files. Every (Designs)

sets the frequency, in design iterations.The Max. Files Retained sets the limit after which the earliest

existing files are overwritten by the latest.

The files are saved with the following names:

<auto_name>-design-<des_iter>.cas.h5

<auto_name>-design-<des_iter>.dat.h5

<auto_name>-id-<optimization_id>.sens (only when you have defined multiple operating

conditions and/or objectives)

where <auto_name> is the File Name, <des_iter> is a three-digit number corresponding to

the design iteration, and <optimization_id> is a two-digit number corresponding to the ID in

the Objectives group box.

Save Optimal Case and Data Files

This group box provides the Save During the Optimization option; when enabled, a single set of

optimal design solution files is saved and rewritten as necessary (as described previously in the step

describing the Adaptive Value option).The files are saved with the following names:

<auto_name>-design-optimal.cas.h5

<auto_name>-design-optimal.dat.h5

<auto_name>-id-<optimization_id>-optimal.sens (only when you have defined multiple

operating conditions and/or objectives)

where <auto_name> is the File Name and <optimization_id> is a two-digit number corres-

ponding to the ID in the Objectives group box.

If you move the .cas/.dat files to a different location, make sure to move the optimal

.cas/.dat and .sens files (only when you have defined multiple operating conditions

and/or objectives) along with it, and set up the proper File Name for the new location in order

to continue the optimization. The optimal files are needed to restore the optimization. Other-

wise, you can reset the optimizer and continue the optimization.

Note that the Save During the Optimization option can only be disabled if you have disabled

the Adaptive Value option.

Export STL Files (Every Design Iteration)

This group box allows you to set up the automatic exporting of .stl files (for 3D cases only), for

use in other software packages. Every (Designs) sets the frequency, in design iterations.The Export

STL Setting... button opens the Export STL dialog box, where you can select the Surfaces of interest.

The files are saved as <auto_name>-design-<des_iter>.stl, where <auto_name> is the

File Name and <des_iter> is a three-digit number corresponding to the design iteration.

.

.

You can set up commands to be executed during optimization (such as postprocessing commands that

export fields) by clicking the Execute Commands... button in the Calculation Activities group box and

using the Execute Commands Dialog Box (p. ) that opens. For details, see Executing Commands During

the Calculation (p. ). Note that once you have opened this dialog box from Gradient-Based Optimizer

dialog box, the following selections become available in the When drop-down list:

Design Iteration

This specifies that execution of the command is based on the design iteration. It is executed after

the design calculation and before any animation recording, both of which are before the morphing

of the mesh.

Adjoint Iteration

This specifies that execution of the command is based on the adjoint iteration. It is executed imme-

diately before each adjoint advancement step.

Note that unexpected behavior may result if the executed command changes settings for the

adjoint calculation and/or gradient-based optimizer.

. You can set up animations to be recorded during optimization by clicking the Solution Animation...

button in the Calculation Activities group box and using the Animation Definition Dialog Box (p. )

that opens. For details, see Creating an Animation Definition (p. ). Note that once you have opened

this dialog box from Gradient-Based Optimizer dialog box, the following selection becomes available

in the drop-down list next to the Record after every field:

design-iteration

This specifies that the recording is based on the design iteration. It is recorded after the design cal-

culation and the execution of any commands, and before the morphing of the mesh.

For details on playing, saving, and/or reading the resulting animation, see Animating the Solu-

tion (p. ).

. Click the Initialize button in the Calculation group box of the Gradient-Based Optimizer dialog box,

and then click the Optimize button to start the design iterations.The optimizer will proceed until one

of the following conditions is met:

the Convergence Criteria is met for all of the observables

the No. of Design Iterations is reached for this optimizer run

the mesh quality requirements cannot be met

you interrupt the calculation

an error occurs

If you want to continue to optimize the design with revised settings for the observables, operating

conditions, objectives, and/or the Adapted Value option, it is recommended that you either Ini-

tialize the optimizer again or Reset it: the current design solution files will be saved as the optimal

if optimization continues, and (for Initialize) the Curr. Design Iteration will be reset to  and the

optimization history in the monitor plot will be lost.

When the optimization is complete, you can click the Summarize button to print a report of the

results for each design iteration in the console, including the observable values, the expected

changes, whether the flow and adjoint calculations converged, and the mesh quality metrics.

When using the Gradient-Based Optimizer, note the following:

It is a good practice to initially run the optimizer for one design iteration, in order to check if the settings

are proper.

The resulting design will be highly affected by whether or not the flow solver and/or adjoint solver reach

convergence. Auto-adjust controls and blend stabilization strategies are recommended for convergence

of the adjoint solver.

You may want to perform a first round of optimization using lower accuracy settings, and then switch to

higher accuracy settings as you approach the optimal solution. For the first round you could consider using

– settings (for example, in the Solution Method task page) that help flow convergence and/or reduce the

residual oscillation

– a coarser mesh

If you change the settings during the optimization (which can change an observable value), you should

make sure to initialize or reset, so that the optimizer considers the current solution to be optimal and starts

the optimization from the current solution; otherwise, the changed observable value may be worse than

in previous calculations, and if the Adaptive Value option is enabled, Fluent will restore the saved optimal

solution and continue, which will undo your settings changes.

The mesh morpher/optimizer offers a variety of non-gradient-based optimization algorithms to optimize

the geometric shape of a system [] (p. ). The optimization can be performed for a wide variety of

physics and quantities of interest to be optimized.

...The Optimization Process

... Optimizers

Note the following limitations of the ANSYS Fluent mesh morpher/optimizer:

The mesh morpher/optimizer should not be used with dynamic or sliding mesh problems.

Any geometrically evaluated parameters required for flow iterations (for example, view factors for

the surface to surface (S2S) radiation model) will need to be recomputed at the very least when the

optimization is complete. If the objective function is affected by one of these geometrically evaluated

parameters, then such parameters will need to be recomputed after each design change; for example,

the view factors need to be recomputed after each design change when the objective function is

Arbitrarily shaped deformation regions are not supported.

All optimization problems require that you identify parameters that can be modified in order to reach

the optimized solution. In the case of the mesh morpher/optimizer, it is the geometry that must be

parameterized. Geometric parameterization for general shapes used in CFD can be very complicated,

due to the large variety of shapes available in engineering applications. In order to minimize such

complications in your ANSYS Fluent simulation, the problem of shape parameterization is reduced to

a problem of the parameterization of changes in the geometry.

The next essential requirement for mesh morphing is a tool that can smoothly alter the shape, irre-

spective of the underlying mesh topology. In ANSYS Fluent, designated deformation regions are ma-

nipulated via displacements applied to a set of control points. The mesh region that is to be deformed

is defined by a “box” (that is, a rectangle for 2D cases and a rectangular hexahedron for 3D), and the

control points must be located within the box. The displacements of the control points are the result

of user-defined motions (each of which involves a parameter value and other directional settings) and

these displacements are then applied to the mesh as a smooth deformation by either interpolating

the displacement based on radial basis functions or using the tensor product of Bernstein polynomials.

The next requirement is to have an optimizer that is robust enough to handle a wide range of problems.

By coupling such optimizers with your CFD analysis, you can greatly improve your design with minimal

intervention. You can use built-in optimizers to vary the parameter values along the prescribed directions

and within defined bounds, in order to satisfy a condition specified by an objective function. The mesh

morpher/optimizer provides you with access to six optimizers that are not based on gradients. Otherwise,

you can manually specify the deformation (that is, define both the parameter values and the directions)

and analyze the results; you also have the option of using Design Exploration in ANSYS Workbench to

easily explore the impact of a variety of parameter values.

The built-in optimizers used as part of the mesh morpher/optimizer capability in ANSYS Fluent use

direct search methods for optimization. Direct search methods are zeroth order, as they only use the

objective function values for optimization. The direct search methods do not use the derivatives.

The following is a list of advantages of direct search methods:

Direct search methods do not require derivatives for optimization.

Direct search methods are robust for problems with discontinuities and in situations where the deriv-

ative computation is not possible or unreliable.

The following is a list of disadvantages of direct search methods:

Convergence proof is not clearly defined.

The rate of convergence can be very slow.

General explanations of the six different built-in optimizers are provided in the following sections:

....The Compass Optimizer

....The NEWUOA Optimizer

....The Simplex Optimizer

....The Torczon Optimizer

....The Powell Optimizer

....The Rosenbrock Optimizer

In the Compass optimizer [] (p. ), the parameters are adjusted one by one until the objective

function is minimized. This optimizer starts with a given value and then evaluates the function value

in all the basic directions. The direction here refers to the positive and negative increments to the

initial parameter values. If there is a reduction in the function value, then that point becomes an im-

proved point. If there is no improvement in the function values, then the step length is reduced by

half and the search is repeated in all directions. The algorithm terminates when the step size falls

below a certain tolerance.

The Compass optimizer initially makes rapid progress towards the solution. While this method might

quickly approach the minimum value of an objective function, it may be slow to detect this fact. It

may also converge very slowly if the level sets of the objective function are extremely elongated.

The NEW Unconstrained Optimization Algorithm (NEWUOA) optimizer [] (p. ) attempts to find

the least value of a function

, where  is a parameter vector of  dimensions. At the start of

every iterative step, a quadratic model approximation (

) is constructed and the minimization is

performed on a trust region (that is, a region around the parameter that is limited by an initial para-

meter variation). The perturbation to the parameter value needed to obtain the lowest value of

is

The Mesh Morpher/Optimizer

evaluated during the iteration, and correspondingly, the new least value of

is obtained. The it-

erative process continues until the trust region is reduced to the optimizer convergence criterion,

and the optimizer exits with the least value of the objective function. This optimization algorithm

can be applied to any setup case of the mesh morpher/optimizer.

The NEWUOA optimizer provides the least value of the objective function in a manner that is highly

accurate and robust. The main advantage of this optimizer is that it is very fast; hence, this optimizer

is recommended for problems that have a large number of parameters.

The Simplex optimizer is also referred to as the Downhill Simplex optimizer [] (p. ), [] (p. )

and the Nelder-Mead method [] (p. ). It is based on the idea of geometric simplexes; for example,

a 2D simplex is a triangle, and a 3D simplex is a tetrahedron.

For optimization purposes, ANSYS Fluent requires that simplexes are regular polyhedra (that is, not

degenerate polyhedra with collapsed sides). Each vertex of the geometric simplex represents one

function evaluation (which in this case is one CFD run), and the number of vertices corresponds to

the number of parameters. For the free-form deformation method that is used by ANSYS Fluent to

parameterize changes in shapes, the number of active control points will determine the number of

vertices of the geometric simplex.

Minimization of the objective function is performed based on a set of the rules about the “quality”

of each vertex. The vertex quality is the value of the function evaluated for each position of the control

point. A set of geometric operations such as reflection, expansion, contraction, and shrinking are

performed in order to find the region in which to look for the minimum of the function. Because

optimization here is formulated as a minimization problem, the simplex optimizer algorithm seeks

the “worst” vertex, that is, the vertex that has the largest value when the corresponding parameter

is evaluated. By performing the reflection around the center of the gravity, the new value of the

function is obtained after performing the CFD run. Similarly, the operations of expansion, contraction,

and shrinking are used to obtain the minimum of the function.

The Simplex optimizer is known to work well, but it suffers from the large number of function evalu-

ations. It also requires smooth objective functions for convergence.

The Torczon optimizer [] (p. ) is a slightly modified version of the simplex optimizer described

previously. Given an initial vertex, this optimizer tries to find a better vertex that has a function value

that is strictly less than the function value at the previous best vertex. There are three possible trial

steps: the rotation step, the expansion step, and the contraction step. The algorithm always computes

the rotation step and then tests to see if a new best vertex has been identified. If it has, then the

expansion step is computed. Otherwise, the algorithm computes and automatically accepts the con-

traction step.

For the Powell optimizer, the method used is based on the number of dimensions of the problem.

For optimization problems of single dimension (that is, problems with a single parameter), the golden

section search algorithm [] (p. ) is used to find the optimal value for the objective function. In

this algorithm, the optimal value is found by reducing the size of the bracketing triplet, until the size

of the bracket (that is, the distance between the outer points of the triplet) reaches a certain tolerance

level. In all the cases, the middle point of the new triplet is determined to be the best value obtained

so far.

For multidimensional problems (that is, problems with multiple parameters), the minimum value and

so far.

the largest decrease is found using the golden search algorithm for each dimension, in order to find

the conjugate directions. A conjugate direction is a direction that when searched will not alter the

minimum value attained by the previous movement in another direction—that is, a direction in which

the gradient is perpendicular to the first direction. After finding the N linearly independent, mutually

conjugate directions, one pass will find the exact minimum value. For functions that are not quadratic,

repeated cycles of N line minimizations will converge to minimum.

In the Rosenbrock optimizer [] (p. ), after the initial direction is found, multiple steps are taken

in that direction until the least value is attained. The process starts with an arbitrary length . If this

initial step succeeds (that is, the new value of the function is less than or equal to the old value), the

length  is multiplied by , where  is more than . If the steps fails, the length  is multiplied by ,

where  is between - and . The direction or the parameter that must be modified is determined

by advancing all the parameters by the step length  and then selecting the best among those that

yield a function value that is less than the previous value. After that point is accepted as the best

point, the process is repeated. These steps continue to repeat until  becomes so small so that any

further change in the value of  does not significantly reduce the value of the function.

The procedure for setting up and using the mesh morpher/optimizer for shape optimization is as follows:

. Read the case into ANSYS Fluent.

. If you want to use one of the built-in optimizers rather than specifying the deformation manually or using

Design Exploration in ANSYS Workbench to explore multiple deformation scenarios, you will need to

provide an objective function in one of three ways: either as a user-defined function (UDF), a Scheme source

file, or a customized function that is based on output parameters (that is, values from flux, force, surface

integral, or volume integral reports).The goal of the optimizer is to deform the mesh in such a way that

this objective function is minimized. ANSYS Fluent will run the solution for a given design stage until con-

vergence is reached, and then check to see if the objective function is satisfied. If the objective function is

not satisfied, ANSYS Fluent will proceed to the next design, and so on, until convergence is achieved from

the point of view of the optimizer.You can specify the optimizer convergence criteria in step .d.iii.

Note that if you plan to use the newuoa optimizer, you must define the objective function as a

UDF.

a.

If you want to provide the objective function as a user-defined function (UDF), perform the steps that

follow. For more information about UDFs, see the separate Fluent Customization Manual.

i.

Write a UDF using the DEFINE_ON_DEMAND macro to define the objective function.The function

name must be objective_function. At the end of the objective function, the rpvar morph-

er/objective_function must be set to the (current - target) value. It is this value

that the optimizer will attempt to minimize.

Using the Mesh Morpher/Optimizer

ii.

Compile the UDF using the Compiled UDFs dialog box. Make sure libudf appears as the Library

Name.

User Defined → User Defined → Functions → Compiled...

b. If you want to provide the objective function as a Scheme source file, perform the following steps:

i.

Write a Scheme source file to define the objective function.The procedure name must be object-

ive-function. At the end of the objective function, the rpvar morpher/objective-function

must be set to the (current - target) value. It is this value that the optimizer will attempt

to minimize.

ii.

Load the Scheme source file (see Reading Scheme Source Files (p. ) for details).

. Open the Mesh Morpher/Optimizer dialog box by clicking Optimizer... in the Design ribbon tab (Para-

meter-Based group box).

The first time you click Optimizer... in a session, a question dialog box will ask you whether you

want to enable the mesh morpher/optimizer. Click Yes to load the libraries and open the Mesh

Morpher/Optimizer dialog box (Figure . : The Regions Tab of the Mesh Morpher/Optimizer

Figure . : The Regions Tab of the Mesh Morpher/Optimizer Dialog Box

. Specify the manner in which you would like to define the locations of the control points, by making

a selection from the Control Point Distribution list in the Regions tab of the Mesh Morpher/Op-

timizer dialog box (Figure . : The Regions Tab of the Mesh Morpher/Optimizer Dialog Box (p. )

and Figure . : The Regions Tab of the Mesh Morpher/Optimizer Dialog Box for an Unstructured

Distribution (p. )). Your selection here will also determine the kinds of motions you can apply to

the control points (in the Deformation tab). You have the following choices:

Regular

For this option, the control points are spread in a regular distribution throughout the entire

deformation region; you only have to define the number of control points along each of the

defining direction vectors. Note that as part of this option, the motion of groups of control

points will have to be defined as a translation, as the ability to define rotational or radial

motions is not available.

Locating control points in this manner is easy and simple, though this comes at the cost of

being able to precisely define control points on specific mesh nodes and boundaries. This

option can be a good choice in cases where you are able to allow the entire mesh within

the region to be deformed—for example, internal flows within a pipe or duct.

Note that as part of this option, the mesh deformation is based on Bernstein polynomials.

While such a direct morphing approach is computationally less expensive than using radial

basis functions, it does not provide you with precise control of a particular mesh node.

Unstructured

For this option, you will define the locations of the control point by right-clicking with the

mouse on boundary zones, distributing an approximate number throughout a zone, or by

entering coordinates. Note that as part of this option, the motion of groups of control points

can be defined as a translation, as a rotation about a point / axis, or radially about a point /

axis.

This option provides great precision with regard to the location of the control points; this

allows you to morph particular nodes and regions of the mesh, as well as to preserve features

within the deformation region (as you can make nodes stationary by applying a parameter

value of zero). This option also allows you to easily define twisting and axisymmetrical motions.

This may be a good choice for external flows and aerodynamic applications.

Note that as part of this option, the mesh deformation is based on radial basis functions.

While this is computationally more expensive than using Bernstein polynomials (because it

involves the solution of a system of equations), it allows you to have precise control of a

particular mesh node if you have created a control point with the same coordinates.

Note that all of the deformation regions that you define in the next step must use the same Control

Point Distribution; if you change this selection at any point, all of the settings in the Regions tab

will be deleted.

Figure . : The Regions Tab of the Mesh Morpher/Optimizer Dialog Box for an Unstructured

Distribution

. Define the region(s) of the domain where the mesh will be deformed in order to optimize the shape,

by performing the following steps. Each deformation region will be defined as a “box”, that is, a

rectangle for 2D cases and a rectangular hexahedron for 3D cases.

Important

Important

It is recommended that you define each deformation region to be bigger than the area

of interest, in order to maintain proper continuity between deforming and non-deforming

regions.

a.

In the Regions tab, enter a name for a deformation region in the text-entry box at the top of the Name

group box.

b. You have the option of using the boundary zones to create a bounding box for the deformation region;

this box can represent the final scope of the region, or it can act as a starting point that is further refined

by manually editing the origin, direction vectors, and size of the region (as described in the steps that

follow). Perform the following steps in the Update from Zones group box:

i.

Select the zones from the Boundary Zones list that best represent the extents of the deformation

region you would like to create.

ii.

Click the Define button in the Bounding Box group box to update the values in the Origin,

Direction- Vector, Direction- Vector (for 3D cases), and Size of Region group boxes.

Note that the bounding box will be previewed in green in the graphics window when you

click any of the Bounding Box buttons.

iii. You can increase or decrease the size of the bounding box by clicking the Enlarge and Reduce

buttons, respectively. Note that you have the option of setting the scaling factors associated with

these buttons via the following text commands:

define → mesh-morpher-optimizer → region → scaling-enlarge

define → mesh-morpher-optimizer → region → scaling-reduce

c.

c.

You have the option of using the line tool (for 2D cases) or the plane tool (for 3D cases) to define the

direction vectors of the deformation region; the values defined can represent the final components of

the vectors, or they can act as a starting point that is further refined by manually editing the direction

vectors (as described in the steps that follow). Set up the line tool or the plane tool (as described in

Using the Line Tool (p. ) and Using the Plane Tool (p. ), respectively), and then click the Update

from Line Tool or Update from Plane Tool button to update the values in the Direction- Vector

and (for 3D cases) Direction- Vector group boxes.

d. Define an origin for the deformation region by entering the Cartesian coordinates of a point in

the X, Y, and (for 3D) Z number-entry boxes in the Origin group box. Note that as you enter

values, you can view the resulting bounding box (in green) by clicking the Preview button.

e. Define the first direction vector of the deformation region relative to the Origin coordinates, by entering

values in the X, Y, and (for 3D) Z number-entry boxes in the Direction- Vector group box.

For 2D cases, ANSYS Fluent will automatically define the second direction vector of the deform-

ation region to be perpendicular to the Direction- Vector, and will display the components in

the uneditable Direction- Vector group box.

f.

For 3D cases, define the second direction vector of the deformation region relative to the Origin co-

ordinates, by entering values in the X, Y, and Z number-entry boxes in the Direction- Vector group

box. If the vector you define is not perpendicular to the Direction- Vector, ANSYS Fluent will automat-

ically redefine the second vector to be the projection of the Direction- Vector you entered onto a

plane that is perpendicular to the Direction- Vector. Based on this definition, the Direction- Vector

you define cannot be colinear with the Direction- Vector.

The third direction vector of the deformation region will be automatically defined as the cross

product of the first and second direction vectors.

g. Define the overall dimensions of the deformation region by entering length values for Direction-,

Direction-, and (for 3D cases) Direction- in the Size of Region group box.

h. Create control points within the deformation region.

i.

If you selected Regular for the Control Point Distribution, define the number of control points

you want along each direction vector of the deformation region by entering values for Direction-

, Direction-, and (for 3D cases) Direction- in the Control Points group box.The total number

of control points for the region will be the product of the numbers you enter. Increasing the number

of control points allows you greater control of the deformation, but also increases the computational

expense.

Important

When you define multiple deformation regions, you must ensure that all the de-

formation regions have the same total number of control points.

Save the settings you have created for the deformation region by clicking the Create button.

The name of the deformation region will be added (and selected) in the selection list at the

bottom of the Name group box, and the control points and bounding box of the deformation

region will be displayed in blue in the graphics window (see Figure . : Displaying the

Control Points for a Regular Distribution (p. )). If you do not want the control points and

bounding box displayed in the graphics window, you can deselect the item by clicking the

button located above the right side of the Name selection list.

Figure . : Displaying the Control Points for a Regular Distribution

A new default name will be automatically entered in the text-entry box at the top of the

Name group box, in preparation for any deformation regions you want to create in the future.

ii.

If you selected Unstructured for the Control Point Distribution, click the Create button to save

the settings for the deformation region, as you need an existing region to be able to create control

points.The name of the deformation region will be added (and selected) in the selection list at the

bottom of the Name group box, and the bounding box will be displayed in blue in the graphics

window (see Figure . : Displaying the Control Points for an Unstructured Distribution (p. )).

If at any point you do not want the bounding box displayed in the graphics window, you can deselect

the item by clicking the button located above the right side of the Name selection list.

Next, examine the settings in the Boundary Continuity group box. By default, the mesh

morpher/optimizer is set to provide smooth mesh transitions wherever the mesh intersects

with the limits of the deformation region (that is, the sides of the bounding box). This is ac-

complished through the creation of stationary control points at those intersections; by default,

these control points are hidden, though you can view them by enabling the Display Control

Points option. If you would like to allow more abrupt mesh transitions at the boundaries of

the region, you can disable the Smooth Transitions option.

The next step is to create control points. Click the Define... button in the Control Points

group box to open the Define Control Points dialog box (Figure . : The Define Control

Points Dialog Box (p. )).

Figure . : The Define Control Points Dialog Box

Use the Define Control Points dialog box to create control points within the region. You

have the following options:

Click the Mouse-Probe button and then probe (using the right mouse button, by default) within

the deformation region. For 3D cases, if you probe on a displayed boundary, the control point

will be located at that point on that boundary. Note that it may be helpful to revise what surfaces

are displayed using the Mesh Display Dialog Box (p. ).

Make a selection from the Zones list, enter an Approximate Number of control points

that you want on that zone, and click the Distribute button. This method uses Binary

Space Partitioning (BSP) to agglomerate the cell faces of the zone within the bounding

box based on the intended number of control points, and then a control point is assigned

to the node that is closest to the centroid of each agglomeration. While this method is

convenient when you want a large number of control points or want to morph entire

boundary zones or surfaces, there are some limitations to BSP: the number of control points

may exceed the value you enter, and the control points will not be as evenly distributed

on curved surfaces when compared to flat surfaces.

Enter X, Y, and Z coordinates and click the Create button.This method allows you to locate a

control point directly on a mesh node, if you have first obtained the vertex position (which can

be displayed in the console if you select long description from the Probe drop-down list in the

View tab (Mouse group box) and then probe near the node with the mouse).

If you have previously generated an ASCII text file that contains control point definitions, you can

read it by clicking Read... and using the dialog box that opens. Using a text file can be helpful

when you have a large number of points. It is not necessary to create the text file from scratch,

as you can create a simplified text file with sample data using the Write... button, and then define

the bulk of the control point locations using a spreadsheet program. See Mesh Morpher/Optimizer

File Formats (p. ) for details about the format of the text file.

The control points will be displayed in green in the graphics window, and will turn red when

selected in the Control Points selection list. When a control point is selected, you also have

the ability to Delete it, or enter new coordinates and Modify it.

When adding control points, remember that it may be helpful to locate them not only in

areas that you want to deform, but also on features in the deformation region that you want

to preserve (as you can make nodes stationary by applying a parameter value of zero). When

you are done adding control points, click OK to close the Define Control Points dialog box.

Figure . : Displaying the Control Points for an Unstructured Distribution

i.

Create any additional deformation regions as necessary by repeating steps .a.–h.

Important

Overlapping deformation regions are not supported.

j.

If you need to modify a deformation region at any point, select it in the Name selection list, revise the

appropriate settings, and click the Modify button.The updated control points and bounding box will

Important

When modifying an existing deformation region, be sure to click Modify rather than

Create. If you click Create, you will not modify the deformation region, but will instead

create a new one with the modified settings.

k.

If you need to delete a deformation region at any point, select it in the Name selection list and click

the Delete button.

. You have the option of defining constraints on the boundary zones, in order to limit the freedom of partic-

ular zones that fall within the deformation region(s) during the morphing of the mesh.The following options

unconstrained

This option specifies that the boundary zone is completely free to be deformed according to the

assigned parameters. By default, all wall zones are unconstrained.

fixed

This option specifies that the boundary zone is fixed and will not be deformed. None of the zones

are fixed by default.

Important

If you specify one or more fixed boundary zones in a deformation region, you must

ensure that there is at least one unconstrained boundary zone in the region as well.

passive

This option specifies that the nodes of the boundary zone are partially constrained to varying

degrees, based on their proximity to adjacent boundary zones that are fixed. The nodes in a

passive boundary zone behave in a similar manner to the interior mesh nodes, in order to ensure

that there is a smooth transition between fixed and unconstrained boundary zones. By default,

all boundary zones that are not walls (for example, inlets, outlets, symmetry, and periodic

boundaries) are passive.

To define the constraints on the boundary zones, perform the following steps.

a.

Click the Constraints tab (Figure . :The Constraints Tab of the Mesh Morpher/Optimizer Dialog

Box (p. )).

Figure . : The Constraints Tab of the Mesh Morpher/Optimizer Dialog Box

b. To revise the default constraints on the boundary zones, select the zone name(s) from the Zones

selection list in the Constraints group box, and then select either Unconstrained, Passive, or

Fixed from the Option list.

c.

c.

Click Display if you want view the boundary zones selected from the Zones selection list, in

order to verify the zones for which you are defining constraints.

d. Click Summary if you would like to print a list in the console that summarizes the constraint definitions

for all of the boundary zones.

. Begin the deformation definition by defining the parameters.

a.

Click the Deformation tab (Figure . :The Deformation Tab of the Mesh Morpher/Optimizer Dialog

Box (p. )).

Figure . : The Deformation Tab of the Mesh Morpher/Optimizer Dialog Box

b. Enter the Number of Parameters that will be used to define the deformation.This number may be as

low as the maximum number of parameters you will define on a single control point, or as high as the

total number of parameters you will set on all of the control points combined.

c.

If you want to manually specify the deformation or use Design Exploration in ANSYS Workbench

to explore multiple deformation scenarios (rather than using the built-in optimizers), define the

parameter fields in the Parameter Values group box. Note that these fields are only available

when none or workbench is selected from the Optimizer drop-down list in the Optimizer tab.

The value of the parameter defines a magnitude that will then be used along with other direction

settings to define motions that produce an overall displacement for a given control point. The

value will specify a length in meters for translations and radial motions, and will specify an angle

in degrees for rotations; the units here will be used regardless of what units you are using in

the case.

the case.

For each parameter you have the following options:

Enter a constant numeric value. Note that having a parameter with a value of zero allows you to

make a control point stationary.

Use the drop-down menu to define the parameter through an expression or input parameter (for

example, as part of a parametric study managed by Workbench); for details, see Directly Applied

Expressions (p. ) or Creating a New Parameter (p. ), respectively.

When you have finished defining the parameter fields, click the Apply button in the Parameter

Values group box to save the definitions.

d. You have the option of limiting how much each parameter is allowed to deform by defining strict

minimum and maximum values.This can be useful when you need to keep the parameters within a

certain tolerance of the initial design, or when you know in advance that certain designs are impractical.

While this option is typically used with the built-in optimizers, it is available for manual deformation,

so that you can visualize the effects of the bounds and set them interactively. Note that this option is

not available when workbench is selected from the Optimizer drop-down list in the Optimizer tab.

Click the Set Bounds... button in the Parameter Values group box to open the Parameter

Bounds dialog box (Figure . : The Parameter Bounds Dialog Box (p. )).

Figure . : The Parameter Bounds Dialog Box

Select the parameters you want to limit from the Parameters selection list, disable the Unboun-

ded option in the Range group box, and then enter appropriate values for Min and Max.

At any point you can click the Apply button to save your bounds, and you can click the Summary

button to display a summary of the saved bounds in the console. When all of the parameter

bounds are defined to your satisfaction, click the OK button to close the Parameter Bounds

. If you selected Regular for the Control Point Distribution in the Regions tab, perform the following

steps. You will define motion settings for the control points by selecting parameters (which you

defined previously) and specifying the translation direction, thus completing the deformation

a.

Click the Motion Settings... button in the Deformation tab to open the Motion Settings dialog box

(Figure . :The Motion Settings Dialog Box for a Regular Distribution (p. )).

Figure . : The Motion Settings Dialog Box for a Regular Distribution

b. (optional) If you have previously generated an ASCII text file that contains motion settings, you can

read it by clicking Read... at the bottom of the Motion Settings dialog box and using the dialog box

that opens; otherwise, you should proceed to steps .c.–.j. and define the settings using the other

controls in the Motion Settings dialog box.

Using a text file can be helpful when you have a large number of motion settings. It is not ne-

cessary to create the text file from scratch, as you can create a simplified text file with sample

values using the Write... button (as described in step .k. ), and then add the bulk of the motion

settings using a spreadsheet program. See Mesh Morpher/Optimizer File Formats (p. ) for details

about the format of the text file.

Important

Immediately after you read a text file, the Motion Settings dialog box will not display

the applied settings. To begin viewing the applied settings, make a selection from

the Region, Control Points, and Parameters lists, and the associated Translation

Direction will be displayed.

You can then edit the motion settings as necessary (in a manner similar to steps .c.–.g.) and/or

proceed to step .m.

c.

Make a selection from the Region drop-down list in the Motion Settings dialog box.

d. Specify the control points in the current Region to which you want to assign the same motion settings

(that is, the same combination of parameters and direction).You can specify these control points using

one or more of the following methods:

Select the ID numbers from the Control Points selection list.The selected control points will be

highlighted in the graphics window.

Click the Mouse-Probe button in the Selection Tools group box and then click the control points

in the graphics window with the mouse-probe button (which is the right mouse button, by default).

To deselect, select a highlighted control point with the mouse-probe button. As you select the control

points, they will also be selected in the Control Points selection list.

Use the Indexed Grouping group box to select the control points based on their assigned indices.

Each control point has i, j, and (for 3D cases) k index numbers, each of which denote its place in the

sequence (starting at the origin of the region) of control points along the direction-, direction-,

and direction- vectors, respectively (as defined in the Regions tab of the Mesh Morpher/Optimizer

dialog box).You can make selections from the index drop-down lists, and then click the Select button.

In a similar way you can deselect control points using the Deselect button. As you select the control

points, they will also be selected in the Control Points selection list and highlighted in the graphics

window.

For example, consider the case of a 3D region: if you select  from the k drop-down list, the

control points in the second plane perpendicular to the direction- vector (that is, the direction-

–direction- plane) will be selected. If you select  from both the i and j drop-down lists, the

line of control points at the intersection of the first planes perpendicular to the direction-

and direction- vectors will be selected. Making selections from all three drop-down lists will

select a single control point.

e. Make selections from the Parameters selection list, in order to specify those you want to assign (along

with a translation direction) to the selected Control Points. Note that the values associated with these

parameters (as displayed in the Parameter Values group box in the Deformation tab of the Mesh

Morpher/Optimizer dialog box) are irrelevant if you plan to use the built-in optimizers.

f.

Define the Translation Direction that will be associated with the selected Parameters by entering

values for the X, Y, and (for 3D cases) Z directions. Note that you do not need to define a unit vector.

If you use a built-in optimizer, these values will provide the direction of the displacement of the

control point and the optimizer will determine the overall magnitude of displacement. Alternat-

ively, if you specify the deformation manually or using Design Exploration, the values you enter

in the Translation Direction group box will be multiplied with the values of the Parameters

to define the displacement applied to the control points.

g. Click the Apply button to save the motion settings.

h. If you want to apply another set of motion settings to the selected Control Points, repeat steps .e.–.g.

for each additional combination of parameters and direction.

i.

Repeat steps .d.–.h. for each additional set of control points in the current Region to which you want

to assign motion settings.

j.

Repeat steps .c.–.i. for each additional region in which you want to apply deformation parameters

to control points.

k.

If you want to save all of the settings you specified in the Motion Settings dialog box as an ASCII text

file, click Write... and specify a name in the dialog box that opens.You can edit the motion settings in

this text file using a spreadsheet program, and then read it in this or a separate case file, as described

in step .b.

l.

You can display a summary of the motion settings in the console by clicking the Summary button.

m. Click OK to close the Motion Settings dialog box.

. If you selected Unstructured for the Control Point Distribution in the Regions tab, perform the

following steps. You will define one or more motions—which consist of a parameter (defined previ-

ously), direction settings, and the affected control points—and thus complete the deformation

Important

When a single control point is associated with multiple motions, note that the resultant

displacement for each individual motion will be calculated from the original position,

and then the displacements will be summed. This means that the order in which the

motions are created will have no effect on the final location of the control point.

a.

(Figure . :The Motion Settings Dialog Box for an Unstructured Distribution (p. )).

Figure . : The Motion Settings Dialog Box for an Unstructured Distribution

b. (optional) If you have previously generated an ASCII text file that contains motion definitions, you can

that opens; otherwise, you should proceed to steps .c.–.k. and define the settings using the other

Using a text file can be helpful when you have a large number of motions. It is not necessary to

create the text file from scratch, as you can create a simplified text file with sample values using

the Write... button (as described in step .l. ), and then add the bulk of the motion definitions

using a spreadsheet program. See Mesh Morpher/Optimizer File Formats (p. ) for details about

the format of the text file.

You can then either add additional motions (in a manner similar to steps 9c.–.h.) or modify /

delete an existing motion (as described in steps .i. and .j.). When the settings are finalized, you

can proceed to step .k.

c.

To begin defining a new motion, make a selection from the Parameter drop-down list.

d. Make a selection from the Type list, to indicate the type of motion you would like to define.You can

specify that a group of control points undergoes a Translation, a Rotation about a point (for 2D) or

an axis (for 3D), or a Radial motion about a point (for 2D) or an axis (for 3D).

e. Define the motion by entering X, Y, and (for 3D cases) Z values for the following: the Direction used

for translations; or the Axis Origin and (for 3D cases) Axis Direction used for rotations and radial mo-

tions. For Direction or Axis Direction, note that you do not need to define unit vectors.

If you use a built-in optimizer, the values you enter will define the direction of the displacement

of the control point and the optimizer will determine the overall magnitude of displacement.

Alternatively, if you specify the deformation manually or using Design Exploration, the magnitude

will be the value of the Parameter; translation is a special case, in which the values you enter

in the Direction group box are multiplied with the value of the Parameter to define the displace-

ment applied to the control points.

f.

Select the control points to which you want to assign the selected motion.You can either select them

in the Control Points list, or click the Mouse-Probe button and click the control points in the graphics

window using the mouse-probe button (which is the right mouse button, by default).

g. A default name will be generated in the top field of the Name group box, based on the Type and

Parameter of the motion.You can edit this text to make it more descriptive, as necessary.

h. Click Create to create the motion.The name will be added to the selection list in the Name group box.

i.

Repeat steps .c.–.g. for each additional motion that you would like to create.

j.

If you need to modify a motion at any point, select it in the lower selection list in the Name group box,

revise the appropriate settings, and click the Modify button.

Important

When modifying an existing motion, be sure to click Modify rather than Create. If

you click Create, you will not modify the motion, but will instead create a new one

with the modified settings.

k.

If you need to delete a deformation region at any point, select it in the lower selection list in the Name

group box and click the Delete button.

l.

You can display a summary of the motion definitions in the console by clicking the Summary button.

m. If you want to save all of the settings you specified in the Motion Settings dialog box as an ASCII text

in step .b.

. If you want to manually specify the deformation (that is, none is selected from the Optimizer drop-

down list in the Optimizer tab of the Mesh Morpher/Optimizer dialog box), perform the following

steps:

a.

steps:

a.

Click the Deform button to apply the current settings (in the Parameter Values group box and Motion

Settings dialog box) and to display the deformed mesh in the graphics window.The Deform button

allows you to manually specify the deformation.

b. You can click the Check button to print out a mesh check report in the console for the currently displayed

mesh.The mesh check report is the same as that produced by the Check button in the General task

page, as described in Mesh Check Report (p. ).

Important

If you save parameter settings but do not click the Deform button, the mesh check

report will not account for the mesh that is produced from those settings.

c.

Click the Reset button if you want to revert to the original mesh without the deformations that result

from the Deform button.

. If you plan to use the built-in optimizers, you should decide whether you want to disable the general mesh

check that is performed by default immediately after the mesh is deformed in every design stage.The

mesh check that is performed is the same as that initiated by the Check button in the General task page

(see Checking the Mesh (p. ) for details). If any errors are discovered, the mesh is rejected and the next

design stage is attempted.

Disabling the general mesh check allows you to repair the mesh, so that an accurate solution can

be calculated for it. Note that you can set up the mesh repair by entering the appropriate text

commands (as described in Repairing Meshes (p. )) in the Initial Commands text-entry box in

the Optimizer tab.

You can disable the general mesh check by using the following text command:

define → mesh-morpher-optimizer → optimizer-parameters → disable-mesh-

check

. If you want to use the built-in optimizers, define the optimizer settings and initiate the optimization process.

a.

Click the Optimizer tab (Figure . :The Optimizer Tab of the Mesh Morpher/Optimizer Dialog

Box (p. )).

Figure . : The Optimizer Tab of the Mesh Morpher/Optimizer Dialog Box

b. Select an optimizer from the Optimizer drop-down list.The available optimizers are not based on

gradients, and include the following: compass, newuoa, powell, rosenbrock, simplex, and torczon.

For more information about how these optimizers function, see Optimizers (p. ).

c.

Click the Objective Function Definition... button to open the Objective Function Definition dialog

box (Figure . :The Objective Function Definition Dialog Box (p. )).

Figure . : The Objective Function Definition Dialog Box

i.

Make a selection in the Options group box to specify whether the objective function that will be

minimized during the optimization process is a User-Defined Function, a Scheme Procedure, or

a customized function of output parameters as defined by the Custom Calculator.Your selection

should correspond with the actions you took in step .

ii.

If you selected Custom Calculator in the previous step, define the objective function via the GUI

controls in the Custom Calculator group box. As you click the buttons in this group box, text and

symbols will appear in the Function to Minimize text box.You cannot edit the contents of this box

directly; if you want to delete part or all of the function, use the DEL or Clear button, respectively.

You can include output parameters in the definition of the function by making a selection

from the Output Parameters list and clicking Select. If you want to add a new output

parameter to the selection list or check the definition of an existing one, you can click the

Parameters... button and use the Parameters dialog box (as described in Creating Output

Parameters (p. )); be sure to click the Refresh button when you return to the Objective

Function Definition dialog box, so that the Output Parameters list is updated. You can also

use Operators to manipulate the output parameters in the function.

You can click the Apply button at any point to save your function. When it is fully defined,

click the OK button to save your settings and close the Objective Function Definition dialog

box.

d. Define the settings in the Optimizer Settings group box.

i.

Enter a value for Maximum Number of Designs, to specify the maximum number of design stages

the optimizer will undergo to reach the specified objective function. Note that this number is not

the number displayed in the console during the optimization process. Each optimizer undergoes a

certain number of design modifications (called “runs”) before it converges to a design for a particular

design stage.The Run number displayed in the console refers to the actual design modifications

(including the inner loop) irrespective of the optimizer, whereas the Maximum Number of Designs

value is the maximum number of converged designs provided by the optimizer.

ii.

Enter the Maximum Iterations per Design, to specify the maximum number of iterations ANSYS

Fluent performs for each design change.

iii. Enter a number for Optimizer Convergence Criteria, to specify the convergence criteria for the

optimizer.

iv. If you selected the newuoa optimizer, enter a number for the Initial Parameter Variation to specify

how much the parameters will be allowed to vary during the initial calculations.This value is not

intended to define a strict minimum / maximum for the parameters (as is defined by the bounds

specified using the Parameter Bounds dialog box), but should only be large enough to allow the

optimizer to capture the minima. A better estimation (that is, a smaller value) allows the optimizer

to reach convergence faster.

e. By default, the orthogonal quality (as defined in Mesh Quality (p. )) of the initial and every subsequent

mesh is computed, before the related solution calculation is initiated. If the orthogonal quality for any

cell is less than a specified value, the mesh is rejected and Fluent proceeds to the next design stage

(therefore helping to ensure that your solution accuracy is not compromised by poor quality meshes).

These actions are governed by the settings in the Mesh Quality group box.

If you do not want the meshes rejected based on their orthogonal quality, you can disable the

Reject Poor Quality Meshes option; otherwise, specify the minimum orthogonal quality that

must be maintained by every cell by entering a value from – (where  represents the worst

quality) for Minimum Orthogonal Quality. When determining an appropriate minimum value,

you can check the orthogonal quality of the initial mesh (by using the Report Quality button

in the General task page) and then select a value that is sufficiently lower, so as not to reject a

majority of the meshes generated during the optimization process.

f.

You have the option of saving intermediate case and data files during the optimization run, so that you

can restart an interrupted solution in the same or a different Fluent session without increasing the

overall number of design iterations needed to reach convergence.To enable the saving of such inter-

mediate files, define the settings in the Case and Data File Set group box.

i.

Specify the frequency (in number of design iterations) that you want the intermediate case and

data files saved by entering a value for Save Every.The default value is , which specifies that no

intermediate files will be saved. Note that if you selected the newuoa optimizer, the frequency at

which files are saved may not exactly correspond to the number you enter, but should be reasonably

close.

ii.

Specify the maximum number of intermediate files sets you want to retain by entering a value for

Maximum Number Retained. After the maximum limit of file sets has been saved, ANSYS Fluent

begins overwriting the earliest existing intermediate file set. Lower values should be used if you

have limited disk space or you are concerned about saving unnecessary files.

iii. Specify a root name for the intermediate files in the File Name text box.When the files are saved,

the design iteration will be appended to this root name to indicate the point at which it was saved

during the optimization run. An extension will also be automatically added to the root name (.cas

or .dat).You can include a folder path in the filename if you want the files saved outside of the

g. Specify how the solution variables should be treated after the mesh is deformed by making a selection

from the Method list in the Initialization group box:

Select Initialize Data After Morphing to specify that the solution variables should be initialized to

the values specified in the Solution Initialization task page after deformation.

Select Continue with Current Data to specify that the solution variables remain the values obtained

in the previous design stage.This selection will reduce the number of iterations needed to reach

convergence compared to the Initialize Data After Morphing selection. Note that if the solver di-

verges during an intermediate design stage, the solution variables will be initialized and the solution

will be attempted again.

Select Read Data File After Morphing to specify that the solution variables are set to the values

obtained from the data file specified in the Data File Name text-entry box.This selection will reduce

the number of iterations needed to reach convergence compared to Initialize Data After Morphing

selection or (in cases where the solution diverges for an intermediate design stage) the Continue

with Current Data selection. Note that this selection is not available when newuoa is selected from

the Optimizer drop-down list.

h. If you did not select the newuoa optimizer, you have the option of specifying commands that will be

executed during the optimization runs of the mesh morpher/optimizer, via the text-entry boxes in the

Execute Commands group box. A command can be a text command or the name of a command macro

you have defined (or will define), as described in Defining Macros (p. ).You can also enter a series

of text commands and/or macros, as long as they are separated by a semi-colon (;).

During optimization runs, deformation occurs as part of every design iteration. You decide the

specific point during the design iteration that the command is executed:

If you want a command to be executed after the design has been modified, but before ANSYS

Fluent has started to run the calculation for that design stage, enter the command in the Initial

Commands text-entry box. There are no restrictions on the commands that can be entered:

you can enter commands that read saved data, perform FMG initialization, execute an entirely

independent on-demand UDF, or even call a Scheme routine.

If you want a command to be executed after the solution has run and converged for a design

stage, enter the command in the End Commands text-entry box. There are no restrictions on

the commands that can be entered. Examples are commands for postprocessing solution

variables, monitoring contours and vectors of different variables, taking snapshots of each

design change, and so on, at every design stage.

Important

If the command to be executed involves saving a file, see Saving Files During

the Calculation (p. ) for important general information.

As noted in Automatic Numbering of Files (p. ), the special character, %i, can

be used to create unique filenames by including the iteration number. However,

by default, the solution will be initialized after each mesh deformation and the

iteration count restarted. Therefore, the resulting filename cannot be used to

identify which design stage produced it (that is, the first design stage may con-

verge at  iterations, and then the second design stage may converge at  it-

erations). The time that the file was created is a better way to identify where in

the series of design stages the file was generated. In addition, some files may be

overwritten if two design stages converge in the same number of iterations. Al-

ternatively, if you have selected Continue with Current Data under Initialization

when setting up the optimizer, then the iteration count will not reset and no

duplicate filenames will occur.

i.

If you did not select the newuoa optimizer, you can plot and/or record the optimization history (that

is, how the value of the objective function varies with each design stage). Click the Monitor... button

to open the Optimization History Monitor dialog box (Figure . :The Optimization History Monitor

Dialog Box (p. )) and perform the steps that follow.

Figure . : The Optimization History Monitor Dialog Box

i.

Enable the Plot option if you want to display a plot of the optimization history in the graphics

window indicated in the Window number-entry box. Note that if you want to observe the mesh

deformations during the optimization process, you must make sure that Window is not set to the

ID of the graphics window that is displaying the mesh.

ii.

Enable the Write option if you want to save the optimization history data in a file, and specify the

File Name.

Note that you can display a plot of the optimization history data generated during the last cal-

culation, even if the Plot or the Write options were not enabled during the calculation, as long

as you have not discarded the data using the Clear button. Simply click the Plot button and the

plot will be displayed in the active graphics window.

j.

Click the Apply button to save your optimizer settings.

k.

Click the Summary button to display a summary of the mesh morpher/optimizer settings in the console.

l.

Click the Optimize button to initiate the optimization process. Information about each run (that is,

each design modification) that is generated as part of the production of a design stage will be displayed

in the console, and the deformed mesh for each run will be updated in the graphics window.

If you set up the saving of intermediate case and data files in step .f and your solution is inter-

rupted during the optimization run, you can restart the calculation using the latest intermediate

files. Note that you should not revise the deformation regions or constraint settings for the re-

started mesh.

. If you want to use Design Exploration in ANSYS Workbench to explore multiple deformation scenarios,

define the optimizer settings.

a.

Box (p. )).

b. Select workbench from the Optimizer drop-down list. Note that workbench is only available if you

have launched your ANSYS Fluent session from ANSYS Workbench.

c.

If necessary, revise the default settings in the Mesh Quality group box, as described in step .e. Note

that the design point associated with a poor quality mesh will not be updated in Workbench.

. Click OK to close the Mesh Morpher/Optimization dialog box.

save your case file and close your ANSYS Fluent session.You can then proceed to ANSYS Workbench and

define the design points that will provide the multiple values for the input parameters you created / assigned

in step .c. For more information about using design points to explore ANSYS Fluent results, see Working

With Input and Output Parameters in Workbench in the ANSYS Fluent in Workbench User's Guide.

. If you manually deformed the mesh or used the built-in optimizers, run your case file with the deformed

mesh.

. If you want to rerun a case file in which the mesh has been deformed by the Optimize button in the Op-

mesh.

timizer tab, you should not revise the deformation regions or constraint settings for the deformed mesh.

Chapter : Performing System Coupling Simulations Using Fluent

You can use System Coupling to perform coupled simulations that involve multiple physics solvers,

coupling active co-simulation participants and/or importing static data from an external data source.

For example, you can run ANSYS Mechanical and ANSYS Fluent) in a single analysis and/or import data

from an output file into an ANSYS Fluent analysis.

System Coupling can be used in two different contexts:

System Coupling in ANSYS Workbench: System Coupling is run from the Workbench interface.

Command-Line System Coupling: System Coupling is run from the command line.

Note

For System Coupling cases using Fluent, it is a best practice to run Fluent in double precision.

Additional information can be found in the following sections:

.. Performing System Coupling in ANSYS Workbench

.. Performing Command Line System Coupling

.. Supported Capabilities and Limitations

..Variables Available for System Coupling

.. System Coupling Related Settings in Fluent

.. FSI Setup Recommendations for Fluent-Mechanical Couplings

.. How Fluent’s Execution is Affected by System Couplings

.. Restarting Fluent Analyses as Part of System Couplings

.. System Coupling case with Fluent using Patched Data

.. Running Fluent as a System Coupling Participant from the Command Line

..Troubleshooting Two-Way Coupled Analysis Problems

.. Product Licensing Considerations when using System Coupling

You can perform system coupling in Workbench by connecting a System Coupling component system

to your Mechanical system and to your ANSYS Fluent fluid flow analysis system.

The following is the list of supported coupling participants:

Fluent

Static Structural

Transient Structural

Steady-State Thermal

Transient Thermal

External Data

Connecting the Setup cell from an ANSYS Fluent analysis system to the Setup cell for the System

Coupling component system signals the latter system that the Fluent solver will act as a co-simulation

participant in a coupled analysis. Most of the coupling related settings for your analysis are made

through the System Coupling system’s Setup user interface. The few coupling related settings that

are required in the Fluent setup are described below, in the section System Coupling Related Settings

in Fluent (p. ). Once the coupling setup is complete, the coupled analysis is executed by updating

the System Coupling system’s Solution cell, rather than the same cell in the connected co-simulation

participant systems.

For more information, see Using System Coupling in Workbench and Supported Participants for System

Coupling in Workbench.

Note

In order to have changes made in Fluent systems propagated to downstream System

Coupling systems, save your project, synchronize with Workbench, or close Fluent. This will

ensure that the information passed to System Coupling matches settings in Fluent. If this is

not done, the analysis may be allowed to run but the following Workbench state error will

be issued at the end of the run:

Update of the Solution component in System Coupling failed: Update

of the Solution component in System Coupling did not mark container

as updated (final state is OutOfDate).

Command-Line System Coupling provides enhanced control over coupled simulation processes, including

automatic starts and restarts for participants, the ability to manipulate the System Coupling data model

via command line, and an interactive solution workflow. In this context, you can still set up participant

physics in the participant's user interface, but you'll perform the coupled analysis —starting the coupling

service, loading participants, specifying values for coupling-related analysis settings, and automatically

starting participants— using the command line.

Note

If you don't want to use a fully automatic coupling workflow, you still have the ability to run

one or more participants manually.

The the command-line System Coupling workflow requires a System Coupling participant file (.scp)

written by Fluent, as described in Generating a System Coupling File (p. ).

Once the physics and System Coupling setups are complete, the coupled analysis is executed and

managed by the System Coupling Service.

For more information, see Using Command-Line System Coupling.

Performing System Coupling Simulations Using Fluent

... Generating a System Coupling File

To utilize command-line System Coupling, you must generate a System Coupling participant (.scp)

file.

You can write a .scp file at any time even if you have not specified any System Coupling information

file.

by selecting the Write SCP File... ribbon tab item to open the Select File dialog box.

File → Export → System Coupling... → Write SCP File...

Enter the name of System Coupling participant file and click OK.

You also have the option of automatically writing all available surface and volume information that

could be used in a System Coupling run any time you write a case file.

You can enable this at any time by selecting the Auto-write SCP File... ribbon tab item.

File → Export → System Coupling... → Auto-write SCP File...

On the dialog box that appears, select Auto-write SCP File with Case File and click OK.

Afterwards, any time you write a case file, a .scp file will also be written.

ANSYS Fluent supports the following capabilities when used in a System Coupling analysis:

Force and displacement data transfers on wall boundaries (including walls in sliding mesh zones),

porous jump boundaries, and porous zone interfaces:

– Input of incremental displacements data from System Coupling allow moving and deforming mesh

specification on boundary wall regions (including walls in sliding mesh zones), porous jump bound-

aries, and porous zone interfaces (via a zero-thickness porous jump boundary). Note the additional

System Coupling option in the Dynamic Mesh Zones dialog box; see Specifying the Motion of Dy-

namic Zones (p. ) for more information.

– Output of force data on boundary wall regions (including walls in sliding mesh zones), porous jump

boundaries, and porous zone interfaces (via a zero-thickness porous jump boundary). Fluent is able

to serve the total force variable (viscous and normal) on all wall boundaries (with or without enabling

the System Coupling option in the Dynamic Mesh Zones dialog box). See Variables Available for

System Coupling (p. ) for details about the forces transferred from the wall and porous jump

Thermal data transfers on wall boundaries and cell zones:

– Input of temperature data and heat flow data from System Coupling on all wall boundaries. Note

the additional via System Coupling option in the Thermal tab of the Boundary Conditions dialog

box.

– Input of heat rate data from System Coupling on cell zones.

Supported Capabilities and Limitations

– Output of temperature data, heat flow data, and heat transfer coefficient data to System Coupling

on all wall boundaries (with or without enabling the System Coupling option in the Dynamic Mesh

Zones dialog box).

– Output of temperature data to System Coupling from cell zones.

Data transfers from wall boundaries that are in Fluent sliding mesh zone or rigid body zone.

The use of triangular and quadrilateral faced interface cell types.

Full dynamic mesh support everywhere except on coupling interface.

Full support for local and distributed parallel solver execution.

Convergence data for all equations (for example, continuity, momentum, and energy convergence

data) is shared with the system coupling service at run time. Monitor data is shared if the monitor point

has an iteration frequency set. If the monitor point has a time step frequency set, monitor data will not

be shared with System Coupling.

In Workbench, this data from Fluent can be charted in conjunction with other data in the system

coupling chart at all available intervals. Intermediate data points are not artificially created in

the system coupling chart.

Monitor data can also be plotted in Fluent Solution Monitoring.

Note the following limitations when using Fluent in a System Coupling analysis:

Using System Coupling with the Remote Solver Manager (RSM) in Fluent is not supported. If attempted,

you will receive the following message:

Solution updates for Fluent systems participating in System Couplings

must run in the foreground. This change has been automatically applied.

When using a wall and wall-shadow pair in Fluent as System Coupling interfaces, you'll need to create

a duplicate surface in Mechanical.These will be paired with two sets of shell elements in Mechanical.

For more information, see Coupling with Wall/Wall-Shadow Pairs or Thin Surfaces in the Mechanical

User's Guide.

Fluent must use a 3D mesh, with data transfer regions consisting of element faces within the 3D mesh.

Data Transfer regions cannot exist in 2D meshes (where the data transfer region would be a line/curve).

Data transfer regions on the coupling interface cannot contain hanging nodes (which result from

hanging node adaption and may occur in some CutCell meshes).

The mesh topology on a System Coupling boundary in Fluent must remain fixed for the duration of

the analysis.This means that dynamic remeshing cannot be used on the System Coupling boundary,

but interior nodes away from the System Coupling boundary can still be remeshed during the solution.

To transfer forces on wall and wall-shadow pair, you need two surfaces in Mechanical to match the two

surfaces in Fluent. In this case, you cannot use a single set of shell elements in Mechanical. An example

of a wall and wall-shadow pair is two different fluids on either side of a zero-thickness internal wall in

Fluent.

The non-iterative time-advancement (NITA) scheme in Fluent cannot be used in a System Coupling

analysis.

When executing design points for System Coupling cases where Fluent is a participant, Program

Controlled should not be used for Fluent Initialization Method.

Shell conduction is not available when the Fluent region is set up to receive thermal data via System

Coupling.

The following variables will be available on all boundary wall regions.

Table . : Variables On Boundary Wall Regions

Physical

Type

Data Type

Transfer

Direction

Display Name / Internal Name

Force

VectorXYZ*

Output

force / force

Length

Input

displacement / displacement

Scalar

Input

and

Output

temperature / temperature

Heat Rate

Scalar

Input

and

Output

heat flow / heatflow

Heat

Transfer

Scalar

Output

heat transfer coefficient / heat-

transfer-coefficient

Scalar

Output

near wall temperature / near-

wall-temperature

The following variables will be available on all cell zone regions.

Table . : Variables On Cell Zone Regions

Physical

Type

Data Type

Transfer

Direction

Heat Rate

Scalar

Input

heat rate / heatrate

Scaler

Output

The following variables will be available on all porous jump boundaries.

Heat Rate

Scalar

Input

Scaler

Output

Table . : Variables On Porous Jump Boundary

Physical

Type

Data Type

Transfer

Direction

Force

Output

Length

Input

Represents the force vector  (

,

,

) and the displacements vector  (

,

,

) respectively.

Variables Available for System Coupling

For information on the data transfers supported by System Coupling for each participant in each

coupling context, see the tables in System Coupling Capabilities.

... Force transferred to System Coupling from a Wall Boundary

The force vector sent from each wall boundary in Fluent to System Coupling is given by:

(.)

where

is the gauge pressure in Fluent.

is the pressure rise due to Floating Operating Pressure if enabled (for details, see Floating Operating

Pressure (p. )).

is the Reference Pressure, which differs from the Operating Pressure (for details, see Reference

Values (p. )). If the Reference Pressure is set to zero, then gauge pressure forces will be sent to System

Coupling. If it is set to the negative of the operating pressure, then absolute pressure forces will be sent

to System Coupling.

is the face area vector.

is the force vector due to viscous forces.

is the force vector due to particle forces.

Note

If buoyancy is active, the hydrostatic pressure force due to a nonzero operating density is

excluded from the force calculation. To include this contribution, the operating density

must be set to .

For more information on force calculations, see Computing Forces, Moments, and the Center of Pressure

... Force transferred to System Coupling from a Porous Jump Boundary

When a porous jump boundary is selected as a source region for a system coupling analysis, the forces

transferred from this porous jump boundary are calculated differently depending on if the porous

jump is between fluid regions, or between a fluid region and a porous zone.

When the porous jump separates two fluid zones, or forms an interior region in a fluid zone:

The force transferred to System Coupling is the net force across the jump. The thickness and

coefficient parameters defined for the porous jump are used to calculate the pressure drop

across the jump. This pressure drop is converted to a force vector that is transferred to System

Coupling. This force does not include any viscous forces.

When the porous jump separates a porous zone and a fluid zone:

This case will occur if the upstream or downstream fluid-porous interface is changed to a porous

jump. The porous jump is used to allow a connection between the upstream and downstream

porous zone interface and System Coupling, since the porous zone interface regions cannot

connect directly to System Coupling.

The face pressure on the porous jump is converted to a force vector and transferred to System

Coupling. A positive face pressure will produce a force vector that always points into the porous

zone. The force calculated does not include any viscous forces.

It is best to assign zero-thickness to the porous jump so that there is no pressure drop across

the jump. Note that volumetric forces in the porous zone are not passed to System Coupling.

This case is intended to model thin porous zones where the deformation of the zone can be

approximated by considering only the fluid pressure on the upstream and downstream porous

interfaces.

If a nonzero thickness is assigned to a porous jump that is adjacent to a porous zone, then

there will be a pressure drop across the porous jump. The force transferred to system coupling

is calculated using the face pressure on the upstream side of the porous jump, before the

pressure drop across the jump has been applied. See the image below.

– Force transferred on the upstream side of the porous zone (a) will be consistent with the

upstream fluid pressure (a).

– Force transferred on the downstream side of the porous zone (c) will be inconsistent with

the downstream fluid pressure (d). On the downstream side of the porous zone, the force

transferred to system coupling is consistent with the exit pressure from the porous zone,

before the pressure drop across the porous jump has been applied. The downstream fluid

pressure is calculated after the pressure drop is applied.

Figure . : Force transferred to System Coupling when Porous Jump Thickness is

Non-Zero

For information about the porous jump boundary condition, see Porous Jump Boundary Condi-

... Displacement transferred from System Coupling

The following applies in a coupled analysis where displacement is received by Fluent.

The displacement data received by Fluent represents the incremental displacement for the current

time step (the incremental displacement since the end of the previous time step).

The displacement variable is only available on walls that have the System Coupling moving and de-

forming mesh (MDM) option selected, and that qualify as valid coupling regions.

In a general coupled analysis, when Fluent solves before or simultaneously to the solver sending the

displacement (such as Mechanical), then during the first coupling iteration of each coupling step the

displacement received is  [m].

... Displacement transferred from System Coupling to a Sliding Mesh

Zone

When transferring data to or from a wall boundary in a sliding mesh zone, you must ensure that the

coupled participant (such as Mechanical) does not rotate its mesh. One way to do this in Mechanical

is to use a Rotational Velocity.

For more information about the Rotational Velocity boundary condition, see Rotational Velocity in the

Mechanical User's Guide. For information about sliding meshes in Fluent, see Using Sliding Meshes (p. ).

... Absolute Pressure Example

Force transferred from a Fluent wall boundary in a System Coupling analysis is the gauge pressure

minus the specified Reference Pressure. You can change the force transferred by changing the Reference

Pressure value. The following example of a pressurized sub-sea pipe is a demonstration of how to

transfer the absolute pressure in a System Coupling analysis by changing the Reference Pressure.

Consider flow in a pressurized sub-sea pipe. The pipe is pressurized to  bar absolute and the exter-

ior water pressure is  bar. The exterior sea water is not modeled. The internal surface of the pipe

forms an FSI interface to a Mechanical model of the pipe.

In Fluent the Operating Pressure would typically be set to  bar. By default the forces passed to

System Coupling would only include the local pressure changes relative to  bar, which clearly does

not represent the real physics. To include the absolute pressure in the forces sent to System Coupling,

the Reference Pressure in Fluent should be set to - bar. The Mechanical model would then need a

pressure of  bar applied to the exterior surfaces of the pipe.

Although this approach is valid, it is not ideal because the correct structural solution is only obtained

if  bar of the interior pressure cancels out with the  bar exterior pressure. Relying on two large

forces to exactly cancel out is prone to discretization (mesh resolution) errors. Minimizing the forces

sent across the FSI interface is also good practice. Therefore the best approach is to use an Operating

Pressure of  bar and a Reference Pressure of - bar in Fluent. The forces Fluent sends to System

Coupling are then based on the gauge pressure minus - bar, that is, the gauge pressure plus  bar.

This accounts for the pressure difference between the interior and exterior of the pipe, so there is no

need to apply an external pressure in Mechanical. We are no longer relying on two large forces cancelling

out and we have minimized the forces sent across the FSI interface.

Double-Precision Solver

System Coupling cases may benefit from the use of Fluent's double-precision solver. For coupling

cases with moving and deforming meshes (MDM), it is a best practice to use Fluent's double-precision

solver. For more information about Fluent's single- and double-precision solvers, see Single-Precision

and Double-Precision Solvers in the Fluent User's Guide (p. ).

– In the Fluent Launcher, select Double Precision to use Fluent’s double-precision solver.

– The System Coupling option must be selected on the desired moving and deforming wall

boundaries in order to obtain displacements from other co-simulation participants taking part in

the coupled analysis.

– Make sure the appropriate solution stabilization options are selected in the Solver Options

tab for the System Coupling boundary zone (and possibly other boundary zones nearby).

Solution stabilization should be activated if you find that the Fluent solution is particularly

sensitive to the data obtained through system couplings. For example, it is often beneficial

for FSI problems in which the fluid is incompressible.

Heat Transfer

– The via System Coupling option must be selected on the desired wall boundaries in order to obtain

heat transfer data (temperature or heat flow) from other participants taking part in the coupled

analysis.

– When running as part of a transient coupled analysis, the step size for and duration of the analysis are

analysis.

controlled by the System Coupling service.

→ The Time Step Size specified in the Fluent setup is currently ignored; the Fluent solution will be advanced

using the time step size specified as part of the System Coupling setup.

→ The Number of Time Steps is also ignored.

– The specified Max Iterations/Time Step corresponds to the maximum number of nonlinear solver iterations

performed per coupling iteration.

For steady-state, system–coupled Fluent analyses, the number of iterations specified in Fluent is equal

to the maximum number of solver iterations solved per coupling iteration in a coupling step. Prior to

ANSYS FLUENT ., the number of iterations specified in Fluent was equal to the solver iterations

solved in a coupling step and was divided equally between the coupling iterations in a coupling step.

You can recover the previous behavior by using the following command: (rpsetvar

’sc/steady/default-iteration-method? #f).

For pseudo-transient cases, refer to Performing Pseudo Transient Calculations (p. ) in the Fluent User's

For steady-state dynamic mesh applications, refer to Steady-State Dynamic Mesh Applications (p. )

System Coupling Related Settings in Fluent

The following are best practices for FSI (fluid-structure interaction) cases involving Fluent and Mechan-

ical:

... Using Contact Detection for Fluent-Mechanical FSI Problems

... Recommendations for Dynamic Mesh Settings for Fluent-Mechanical FSI

... Pathologies & Candidate Resolutions for Fluent-Mechanical FSI

In general terms, contact detection determines where the computed mesh motion will result in contact

of a moving surface with other surrounding surfaces. However, the Mechanical and Fluent solvers each

define it a bit differently. For Mechanical, it refers to surfaces/bodies coming into physical contact,

while for Fluent, it refers to what Fluent does when two surfaces come into close proximity (i.e., flow

blockage).

Contact detection is often used in FSI simulations requiring flow blockage – i.e., cases for which you

need to restrict the flow or limit the movement between boundaries – such as valve applications with

highly flexible flow-control geometry. Using the same geometry, you can apply an offset to both the

fluid and structural sides of the analysis. The offset applied in Fluent specifies a tolerance within which

cells are flagged for the application of flow resistance, while the offset specified in Mechanical (as de-

scribed in Geometric Modification in the Mechanical User's Guide) restricts the moving boundary by a

certain distance from a surrounding surface, so that a flow restriction can be applied in that cavity.

This also prevents the fluid mesh from folding if the mesh is pinched between the moving boundary

and a surrounding surface. The offset applied to the structural side is intended to mirror the movement

restriction applied on the fluid side, so that both bodies are aligned during coupling. This simplifies

the process because no modification to the geometry or mesh is required.

The recommended sequence for setting up contact detection in a coupled FSI problem between a

Fluent-Mechanical coupling is summarized below:

. Set up contact detection in the Fluent solver.

a.

Identify the distance that will be required to block off the flow. (To do this, you may need to run one-

way FSI analysis to test how close the moving boundary can get to surrounding surfaces without

causing the mesh to fold.)

b. Using the obtained distance, set the contact detection tolerance — i.e., a proximity threshold to detect

when the moving boundary is within a specified tolerance of the surrounding surface.

c.

Apply viscous or porous resistance to restrict the flow between the offset, using the flow-control settings

provided by the Fluent solver.

For more information, see Contact Detection Settings (p. ).

. Set up contact detection in the Mechanical solver.

In the structural solver, configure contact detection settings to match those of the Fluent solver.

For more information, see Geometric Modification in the Mechanical User's Guide.

FSI Setup Recommendations for Fluent-Mechanical Couplings

... Recommendations for Dynamic Mesh Settings for Fluent-Mechanical

FSI

Smoothing

Diffusion-based smoothing is generally recommended, using the boundary distance diffusion function.

A diffusion parameter (α) = . is a good starting point, as it works well for absorbing the motion with the

far field mesh.

If the boundary layer mesh deforms, increasing the diffusion parameter can further preserve the mesh

close to the moving boundary.

If remeshing is not required Smoothing From Reference Position should be selected, specifically for

periodic motion.

Remeshing

Recommended starting point for the remeshing minimum (Lmin) and maximum length scales (Lmax) are

.4Lmin and .4Lmax.

– Global length scales can be set through: Dynamic Mesh > Settings > Remeshing > Parameters.

– Global length scales of the mesh can be found in Mesh Scale Info.

– Local length scales can be found for each Dynamic Mesh Zone under the Meshing Options tab

Remeshing and smoothing should be enabled locally for all Dynamic Mesh Zones that are of type Deforming,

this allows remeshing and smoothing to be applied to faces adjacent to the System Coupling Region.

– In addition, both Region and Local should be selected for Remeshing Methods. Region allows remeshing

based on length scales while Local allows for remeshing based on skewness. It is important to note that

remeshing will not occur if Local is not selected.

It is also important to remember that there is no direct control over skewness and size criteria of the

remeshed cells. Therefore, you can only indirectly control these criteria of the deformed mesh. For that

reason, if the remeshed cells are not of adequate quality, the user can further tighten the related cri-

teria.

Troubleshooting information is available on the following topics:

.... Mesh Folds within the First Coupling Steps

.... Deformed Prism Layers

.... Interior Elements have High Skewness or Are Too Large/small

. Identify where the mesh folding is occurring.

Open case file for the folded mesh and examine the Cell Volume contour for the domain. You can

highlight the folded cells by setting the maximum range to , so that only cells with a negative

volume are displayed. This can give an indication of what might be causing the mesh folding —

i.e., the time step size might be too large, or the dynamic zones may be set up incorrectly. For

information on how to address cases where the prism layer is folding, see Deformed Prism Layers

(p. ).

. Rerun the case with smoothing and remeshing verbosity turned on.This may provide clues as to what

is causing mesh folding.

a.

To turn on verbosity for smoothing, enter the following command into the Fluent TUI:

/define/dynamic-mesh/controls/smoothing-parameters/verbosity

b. To turn on verbosity for remeshing, enter the following command into the Fluent TUI:

(rpsetvar 'dynamesh/remesh/verbosity )

Note

If remeshing is not triggered, verify that the Dynamic Mesh Zones and length scales are

set up correctly

. Open the case file for the folded mesh.

. Check the minimum and maximum length scales for the mesh and compare these to the

remeshing values.

. If needed:

Tighten the length scales and skewness factors.

Increase the Size Remeshing Interval value.

A deformed prism layer can quickly cause a case to fail due to the mesh folding. Fluent currently does

not support the remeshing of prism layers. If a case exhibits deformation in the boundary layer due

to large movement/deformation of the FSI regions, there are three main recommendations that de-

pending on the case can resolve this pathology:

. Increase the Diffusion Parameter to increase the mesh stiffness around the boundaries and cause regions

away from the moving boundary to absorb more of the motion.

. If the prism layer mesh around the moving body is uniform (i.e. constant number of prism mesh layers

around the geometry), it is recommended to split the boundary layer mesh into a separate Cell Zone.

. If the prism layer is not uniform (i.e. stair stepping due to small gaps) and/or contact detection is required

in Fluent, the use of overset meshing is recommended. Overset meshing is also recommended for complex

topologies.

..... Using Boundary Layer Smoothing and Region Face Remeshing

For cases that exhibit prism layer deformation/shearing, i.e. due to translational movement between

two bodies in close proximity as shown in Figure . : Skewed prism cells due to translational motion

between two bodies in close proximity  (p. ) below; boundary Boundary Layer Smoothing Meth-

od (p. ) can be implemented along with Region Face Meshing. Boundary Layer Smoothing pre-

serves the boundary layer by applying the displacement vectors on the coupled face zone to the

nodes of each cell in the boundary layer zone. This requires that the boundary layer mesh is split

into a separate zone. As an example, we will go through the procedure of splitting the boundary

layer mesh for the geometry shown below (Figure . : Example geometry (p. )). As the geometry

includes a prism layer mesh on the outside walls as well as the inside walls, they will need to be

separated individually. It is important to note that Boundary Layer Smoothing is only applicable

when using Spring-based Smoothing.

Figure . : Skewed prism cells due to translational motion between two bodies in close

proximity

Figure . : Example geometry

Split the prism layer cap to a separate cell zone condition to allow Region Face remeshing to be in-

voked:

. Create a Boundary Cell Register with the required prism elements.

a.

Right click Solution>Cell Registers>New>Boundary

b. Use Cell Distance and highlight the boundary zone were the prism layers are located.The number

of cells is set based on the number of prism layers.

. Use the Boundary Cell Register to separate the prism layers into a separate cell zone.

a.

Click Zones > Separate > Cells.

b. Select the register with the prism cells and the zone that you’d like to split.

. Verify that the correct cell zones were created based on the cell registers and zones.

In this case we have split our single cell zone into three separate cell zones. The first cell zone

contains the inner boundary layer mesh (Figure . : Cell Zone containing the inner boundary

layer mesh (p. )), the second cell zone contains the outer boundary layer mesh (Figure . : Cell

Zone containing the outer boundary layer mesh (p. )) and finally the third cell zone contains

the interior mesh (Figure . : Cell Zone containing the inner boundary layer mesh (p. )).

Figure . : Cell Zone containing the inner boundary layer mesh

Figure . : Cell Zone containing the outer boundary layer mesh

Figure . : Cell Zone containing the interior mesh

. For the Dynamic Meshing settings, select Spring based smoothing as all other smoothing methods do

not support Boundary Layer Smoothing (Deform Adjacent Boundary Layer with Zone) will not be

. Turn on Region Face remeshing.

. Turn off smoothing for the symmetry/wall regions.This prevents cells adjacent to moving wall from

getting too stretched. Smoothing would still be conducted in the interior cells.

. In the Dynamic Mesh Zones, set the moving prism layer cell zone as a rigid body:

a.

By default, Rigid Body Dynamic Mesh Zones require a UDF to specify the mesh motion. Since the

motion is provided by System Coupling, assign a “dummy UDF."

b. The dummy UDF is an empty UDF, as follows:

DEFINE_GRID_MOTION(dummy_motion, domain, dt, time, dtime)

{

return;

}

. For the boundary layer mesh to move with the Coupled region, Deform Adjacent Boundary Layer

with Zone must be turned on:

Setting the Cell Height in the Adjacent Zone is not required, since the prism layer mesh will not be

remeshed.

. Set the Cell Zone containing the interior mesh as Deforming, this will allow the tri/tet faces and cells

(Figure . : Prism layer mesh quality maintained for large deformations (p. )) to be remeshed.

Running the case again, we can see how the prism layer mesh is maintained using Boundary Layer

Smoothing and only the interior cells are remeshed.

Figure . : Prism layer mesh quality maintained for large deformations

..... Overset Meshes

As previously mentioned, for complex topologies and/or if the prism layer is not uniform (i.e. stair

stepping due to small gaps), the use of overset meshes is recommended. By allowing the user to

have a separate mesh for the background and the components, the remeshing and smoothing

parameters can be controlled for each component mesh. For example, the overset mesh below

(Figure . : Overset mesh generated using  separate meshes (p. )) is created using  separate

meshes. A structured hexahedral mesh is used for the background, while a tetrahedral mesh is used

for the two geometries.

Figure . : Overset mesh generated using  separate meshes

The leading edge of the long rectangle rotates clockwise, creating a small gap between the short

rectangle. If a single mesh was used for this case, the prism layer mesh around the  components

deforms and causes the mesh to fold. This occurs as the prism layer mesh starts to absorb the de-

formation as the gap between the two geometries decreases. By having the components separately

meshed, each components mesh absorbs the deformation in its far field, before mapping it back to

the overset mesh, maintaining the prism layer mesh quality (Figure . : Prism layer mesh quality is

maintained (p. )).

Figure . : Prism layer mesh quality is maintained

The general workflow to setup an overset mesh case is as follows:

. Split and remesh the required geometries.

. Revise the time step size:

Consider the three time scales. Note that the smaller timescale is dominant.

– Simulation

– Mesh deformation

– Overset meshing

calculating the time step should be restricted to cells in the overset overlap region.

It is important to not have large variations in mesh resolution in the motion path that could trigger

large changes in the overset interface as the motion proceeds.The use of grid priorities can minimize

large variations in the overset interface.

. Choose the Overlap Minimization required:

A cell-volume-based method is recommended if the component mesh resolution is fine near walls

and increases gradually away from walls and becomes similar in size to or larger than the background

mesh.

Enter the following command into the Fluent TUI:

define/overset-interfaces/options/donor-priority-method

A boundary-distance-based method is recommended when overlapping meshes have uniform and

nearly identical resolutions.Therefore, it is most suitable when two walls have small distance in

between them.

. Create Overset interface and initialize solution:

The overset mesh is created during initialization; it can be viewed through Results > Graphics >

Mesh by checking Overset under Options

Refer to Diagnosing Overset Interface Issues (p. ) for more information.

For cases where interior cells are skewed due to translational and/or rotational movement (Fig-

ure . : Skewed prism cells due to translational motion between two bodies in close proximity  (p. ))

or remeshing resulting in elements that are too large or small, there are two main recommendations

that depending on the case can resolve this pathology:

. Use tighter criteria for the minimum and maximum length scales as well as skewness. In addition,

decrease the Size Remeshing Interval to  so that remeshing based on size is triggered at every time

step.

. If the previous step was not enough to resolve this, Enable Region Face Remeshing. Region Face

Remeshing will not trigger if a prism layer mesh is located in the same cell zone were remeshing needs

to occur.Thus, the user would need to split the prism layer mesh into a separate cell zone. Refer to the

Deformed Prism Layers section for detailed instructions.

For the case shown below, setting tighter criteria for the minimum and maximum length scales to

remesh every time step was not sufficient to produce a high-quality mesh in the gap (Figure . : Ori-

ginal Mesh (left) and deformed mesh (right) with smoothing and remeshing enabled  (p. )). Since

there is no direct control over skewness and size criteria of the remeshed cells, you can only indirectly

control these criteria of the deformed mesh.

By using Region Face Remeshing, this allows more control over the size of the remeshed cells (Fig-

ure . : Original Mesh (left) and deformed mesh (right) using smoothing and Region Face

Remeshing (p. )). This is done by splitting or deleting the cells directly adjacent to the moving

boundary based on the maximum and minimum length scales only. But as previously mentioned, the

prism layer mesh has to be in a separate cell zone and treated as a rigid body.

Figure . : Original Mesh (left) and deformed mesh (right) with smoothing and remeshing

enabled

Figure . : Original Mesh (left) and deformed mesh (right) using smoothing and Region Face

Remeshing

Note

Overset meshes are not supported by CFD-Post. So, post processing must be handled directly

in Fluent.

For overset meshes, volume integrals are taken over all solve cells in the domain.This results

in double counting where solve cells overlap, leading to errors in volume integrals on overset

meshes.

ANSYS Fluent’s execution is modified slightly to allow the Coupling Service to manage the evolution

of the coupled analysis. For more information, see Process Synchronization and Analysis Evolution.

Go to the section Stops and Restarts of System Coupling Runs for general information on restarting a

coupled analysis and links to context-specific information.

For System Coupling in Workbench: Restarting a Coupled Analysis in Workbench.

For Command-Line System Coupling: Restarting a Command-Line Coupled Analysis Run.

To restart your coupled analysis, you will also need restart information specific to the participants con-

nected to your System Coupling system.

Restarting Fluent Analyses as Part of System Couplings

For details on other participant systems connected to your System Coupling system, see the following

lists of supported systems and references to their corresponding documentation regarding restarts:

Supported Participants for System Coupling in Workbench

Supported Participants for Command-Line System Coupling

... Generating Fluent Restart Files

... Specify a Restart Point in Fluent

... Making Changes in Fluent Before Restarting

... Recovering the Fluent Restart Point after a Workbench Crash

Restarts of a system coupling analysis requires corresponding restart points to exist in the coupling

service and in each of the solvers participating in the analysis.

Fluent will automatically generate the corresponding case and data (cas/dat) files based upon requests

received from the System Coupling service. Note that these files are generated in addition to the restart

points (or results) manually requested via the Autosave Every field in the Calculation Activities task

page within Fluent.

When the Fluent solution is updated (or restarted), the case and data files (.cas and .dat) corresponding

to the current restart point will be used, if it exists. The default restart point is taken from the last

generated case and data files. To specify a different restart point, perform the following steps:

. In the Project Schematic, double-click the Solution cell to open the Fluent interface. Do not double-click

the Setup cell, as this will restore the original mesh and settings.

. Select the File/Solution Files... ribbon tab item to open the Solution Files dialog box with a list of all

available restart points.

. Select the desired restart point. By default, the latest saved restart point is selected. Only one restart point

can be selected, so to be able to select a different restart point, first click the highlighted restart point to

deselect it.

Make sure that you select the restart point that corresponds to the restart points selected for the

System Coupling service and the other coupling participants.

. Click Read to read-in the data for the selected restart point.

. Once the data is read, click Close to close the Solution Files dialog box.

. Close Fluent by selecting the File/Close Fluent ribbon tab item.

In some cases, Fluent setup changes are required to avoid failure of the coupled analysis (for example,

changes to iteration controls, under-relaxation factors, and so on). The settings that are stored in the

case file corresponding to the current restart point will be used for Fluent restarts.

Close Fluent by selecting the File/Close Fluent ribbon tab item. If you are presented with a notification

that the modified mesh and settings will be used for the current run, choose OK to accept and close

the dialog box.

Workbench or one of the components may crash such that restart files are available but they are not

recognized or populated in the Workbench project. If this is the case, you will be able to recover your

project and restart your analysis.

See Restarting a Coupled Analysis in Workbench for the steps needed to recover a coupled analysis

after a Workbench crash. You will also need the information below about Fluent, as well as information

specific to the other participant systems connected to System Coupling. For other participant systems

connected to your System Coupling system, see Supported Participants for System Coupling in Work-

bench for a list of supported systems and references to their corresponding documentation regarding

restarts.

The usual project directory ( ProjectName_files) contains the latest Fluent and System Coupling

results and restart points (these solvers use the live project instead of running in a temporary directory).

Note that the .backup directory contains the original version of any files that have been modified

since the last save. These files are useful to recover the last saved state, but they are not useful for

restarting your analysis.

To recover Fluent’s restart point after a Workbench crash:

.

Double-click the Fluent Solution cell to open Fluent interface.

.

Select the File/Solution Files... ribbon tab item to open the Solution Files dialog box with a list of the

restart points.

.

The Solution Files dialog box will not be populated with the data files written before Workbench crashed,

.

so the correct restart point must be recovered. Select Recover Missing Solution... to recover the latest

case and data files, and to populate the corresponding restart points in the Solution Files at list.

.

Now that the solution files list is populated, select the desired restart point.

By default, the latest saved restart point is selected. Only one restart point can be selected, so to

be able to select a different restart point, first click the highlighted restart point to deselect it.

.

Click Read to read-in the data for the selected restart point.

.

Once the data is read, click Close to close the Solution Files dialog box.

.

Close Fluent by selecting the File/Close Fluent ribbon tab item.

When generated data is cleared from a System Coupling case before a rerun, the data that was specified

using Fluent’s patch option is also cleared. For example, in the Multiphase volume of fluid (VOF) cases,

System Coupling case with Fluent using Patched Data

the patched data that is cleared is the volume fraction information. Fluent needs this patched data to

be able to solve accurately. See Patching Values in Selected Cells (p. ) for more information about

patched data.

For a System Coupling case using patched data, follow the steps below. Note that this workaround will

not work with Design Point updates.

.

Before setting up your case in Fluent, tell Fluent to generate the *.ip file so that if needed, you will have

.

access to patched data.To do this:

a.

In Workbench, select Tools>Options.

b.

On the left side of the dialog box that opens, select Fluent, and then check Enable Generation of

Interpolation File.

.

During Fluent setup, an *.ip file will now be written after initialization of your Fluent system.

.

If you want to do a rerun in Workbench, after completing a System Coupling run, you need to Clear

Generated Data on the System Coupling system’s Solution cell. For the cases that use patched data, you

need to then have Fluent read the *.ip file that was generated in your initial setup so that it has the

correct data.To do this:

a.

From the Project Schematic, open Fluent by double-clicking Fluent’s Setup cell.

b.

Select the File/Interpolate... ribbon tab item. In the dialog box that appears, select Read and Inter-

polate, then click Read... .

c.

Browse to the *.ip file, and then click OK to add have Fluent read this file. In the Interpolate Data

dialog box, select Close.

d.

You do not need to initialize Fluent after reading the *.ip file. Close Fluent and continue with the

rerun of your System Coupling case.

.. Running Fluent as a System Coupling Participant from the Com-

mand Line

System Coupling analyses can be run via the command line using either System Coupling context. To

run ANSYS Fluent as a coupling participant:

For System Coupling in Workbench

System Coupling analyses that are set up in Workbench, as described in Setting Up a Coupled

Analysis in Workbench for a Command-Line Run, can be run from the command line.

– Complete the System Coupling-related settings in Fluent (see System Coupling Related Settings in

Fluent (p. ))

– Generate the case and data files needed to start Fluent

→ Choose Write and Case & Data from the File ribbon tab in the Fluent graphical interface

– Run the Workbench setup from the command line, as described in Executing a Command-Line Run

of a Coupled Analysis Set Up in Workbench.

For Command-Line System Coupling

To both set up and run a coupled analysis from the command line, perform the steps outlined

in Setting Up a Command-Line Coupled Analysis and Running a Command-Line Coupled Analysis.

– For information on how to restart an analysis set up and run from the command line, see Restarting

a Command-Line Coupled Analysis Run.

– For details on alternate workflows and capabilities, see Advanced Workflows for Command-Line

System Coupling.

Note that if Fluent is run in interactive mode, the interface will be locked from when it reports it has

established the connection to the coupling service until when all other coupling participants do the

same.This occurs so that all participants may be synchronized at the Initial Synchronization point. For

information about synchronization points, see Process Synchronization and Analysis Evolution.

The following files, found in the Fluent run directory (FFF/Fluent under a Workbench design point dir-

ectory), may prove useful in troubleshooting coupled analysis problems:

cortexerror.log:This file contains a historical summary of all of the errors that have occurred

during all runs executed in the same run directory.With this in mind, ensure that you are considering

messages corresponding to the most recent run. An example message is: "Update-Dynamic-Mesh failed.

Negative cell volume detected." This indicates that at the date and time noted, the mesh unexpectedly

failed.

solution .log:This file includes information regarding the Fluent boundary conditions at which

data from System Couplings was/is used.This file is never appended, and so it only contains information

from the current run.

solution.trn (or other transcript file):This file contains a complete summary of the current/latest

run's evolution.This is one of the most useful files to determine why the coupled analysis failed.To

generate extensive debug output during the analysis, enter the following command when completing

the Fluent problem setup:

(rpsetvar 'sc/verbosity )

Provide all of these files when submitting a request for service to ANSYS personnel.

The licenses needed for Fluent as part of a System Coupling analyses are listed in the table below. Ad-

ditional licenses may be required for other participant systems in the coupled analysis, but no additional

licenses are required for the System Coupling infrastructure itself.

The simultaneous execution of coupling participants currently precludes the use of the license sharing

feature that exists for some product licenses. The following specific requirements consequently exist:

Distinct licenses are required for each coupling participant.

Product Licensing Considerations when using System Coupling

Licensing preferences should be set to 'Use a separate license for each application’ rather than 'Share

a single license between applications when possible.'

Note

If you are running one of the ANSYS Academic Mechanical and CFD licenses (Associate,

Research, or Teaching) with a solver license that supports license sharing, then you will be

able to run an FSI simulation with a single license.

Table . : Licenses required for Fluent as part of a System Coupling analysis

Academic License Required

Commercial License

Required

System

Fluent

ANSYS Academic Associate

Mechanical and CFD,

ANSYS CFD,

ANSYS Fluent, or

ANSYS Academic Associate CFD,

ANSYS Fluent Solver

ANSYS Academic Research

ANSYS Academic Research CFD,

ANSYS Academic Teaching

Mechanical and CFD, or

ANSYS Academic Teaching CFD

Chapter : Customizing Fluent

You can use ANSYS ACT to create simulation wizards that can be run from either stand-alone Fluent or

Fluent in Workbench. For general ACT usage information, see the ACT Developer's Guide. For information

on ACT usage specific to Fluent, see ACT Customization Guide for Fluent.

Chapter :Task Page Reference Guide

This reference guide provides information about the task pages in Fluent.

.. Meshing Task Page

.. Setup Task Page

.. General Task Page

.. Models Task Page

.. Materials Task Page

.. Phases

.. Cell Zone Conditions Task Page

.. Boundary Conditions Task Page

.. Overset Interfaces Task Page

.. Dynamic Mesh Task Page

.. Reference Values Task Page

.. Solution Task Page

.. Solution Methods Task Page

.. Solution Controls Task Page

.. Solution Initialization Task Page

.. Calculation Activities Task Page

.. Run Calculation Task Page

.. Results Task Page

.. Graphics and Animations Task Page

.. Plots Task Page

.. Reports Task Page

.. Parameters and Customization Task Page

The Meshing task page introduces you to the most common meshing tasks involved in solving your

CFD simulation using ANSYS Fluent.

The Setup task page introduces you to the main tasks involved in setting up your CFD simulation using

The General task page allows you to set various generic problem settings, such as those related to the

mesh or the solver. Note that these settings become available only after you read in a case or mesh

file. See Reading Mesh Files (p. ) and Reading and Writing Case Files (p. ) for details.

Controls

Mesh

contains controls relating to mesh settings.

Scale...

opens the Scale Mesh Dialog Box (p. ).

Check

verifies the validity of the mesh.The check provides volume statistics, mesh topology and periodic

boundary information, verification of simplex counters, and verification of node position with reference

to the  axis for axisymmetric cases. See Checking the Mesh (p. ) for details.

It is recommended that you check the mesh right after reading it into the solver, in order to detect

any mesh trouble before you get started with the problem setup.

Report Quality

displays various quantities related to the quality of the mesh in the console, such as Minimum Ortho-

gonal Quality and Maximum Aspect Ratio. See Mesh Quality (p. ) for details.

Display...

Solver

contains controls relating to solver settings.

Type

contains the solution methods available for computing a solution for your model. See Using the Solv-

er (p. ) for details.

Pressure-Based

enables the pressure-based Navier-Stokes solution algorithm (the default).

Task Page Reference Guide

Density-Based

enables the density-based Navier-Stokes coupled solution algorithm.

Velocity Formulation

specifies the velocity formulation to be used in the calculation. See Choosing the Relative or Absolute

Velocity Formulation (p. ) for details.

Absolute

enables the use of the absolute velocity formulation.This is the default setting.

Relative

enables the use of the relative velocity formulation.This option is available only with the Pressure-

Based solver.

Time

contains options related to time dependence.

Steady

specifies that a steady flow is being solved.

Transient

enables a time-dependent solution. See Performing Time-Dependent Calculations (p. ) for details.

2D Space

contains options available only when solving two-dimensional problems.

Planar

indicates that the problem is two-dimensional. (This option is available only when you start the

2D Space

Planar

2D version of the solver.)

Axisymmetric

indicates that the domain is axisymmetric about the  axis.When Axisymmetric is enabled, the

2D axisymmetric form of the governing equations is solved instead of the 2D Cartesian form. (This

option is available only when you start the 2D version of the solver.) Be sure to change the zone

type of the axis of rotation to axis, using the Boundary Conditions Task Page (p. ), as described

in Changing Cell and Boundary Zone Types (p. ).

specifies that the swirl component (circumferential component) of velocity is to be included in

your axisymmetric model.You should select this option if you are solving swirling flow in an

axisymmetric geometry (see Swirling and Rotating Flows (p. ) for more information).

Gravity

enables the specification of gravity.

Gravitational Acceleration

sets the ,

, and  components of the gravitational acceleration vector. (The  component is available

only in 3D solvers.) See Natural Convection and Buoyancy-Driven Flows (p. ) for details about buoyancy-

driven flows.This option appears only when Gravity is enabled.

Units...

opens the Set Units Dialog Box (p. ).

... Scale Mesh Dialog Box

General Task Page

... Mesh Display Dialog Box

... Set Units Dialog Box

... Define Unit Dialog Box

... Mesh Colors Dialog Box

The Scale Mesh dialog box allows you to convert the mesh from various units of measurement to SI

or to apply custom scale factors to the individual coordinates of the mesh. See Scaling the Mesh (p. )

Controls

displays the Cartesian coordinate extremes of the nodes in the mesh. (These values are not editable; they

are purely informational.)

Xmin,Ymin, Zmin

shows the minimum values of Cartesian coordinates in the mesh.

Xmax,Ymax, Zmax

shows the maximum values of Cartesian coordinates in the mesh.

Scaling

contains controls for converting units and setting the scale factors automatically.

Convert Units

allows you to use the conversion factors provided by ANSYS Fluent.Then indicate the units used

when creating the mesh by selecting the appropriate abbreviation for meters, centimeters, millimeters,

inches, or feet from the Mesh Was Created In drop-down list.The Scaling Factors will automatically

be set to the correct values (for example, . meters/inch).

Specify Scaling Factors

allows you to manually specify a scale factor in each of the Cartesian coordinate directions.

Mesh Was Created In

contains a list of common units of length.The Scaling Factors will automatically be set based on

your selection.The units include common SI and British units such as centimeters (cm), millimeters

(mm), inches (in), and feet (ft).

Scaling Factors

contains the factors applied to the mesh in each of the Cartesian coordinate directions.You can enter

values manually, or use the Mesh Was Created In list to set scale factors automatically.

X

is the scale factor in the  direction.

Y

Z

X

Y

Z

is the scale factor in the  direction (appears only in 3D).

Scale

multiplies each of the node coordinates by the specified scale factors.

Unscale

divides each of the node coordinates by the specified scale factors.

View Length Unit In

contains a list of common units of length.The Domain Extents will automatically be set based on your

selection.The units include common SI and British units such as centimeters (cm), millimeters (mm),

inches (in), and feet (ft).The units of length in the Set Units Dialog Box (p. ) will change each time you

change your selection in the View Length Unit In drop-down list.

The Mesh Display dialog box controls the display of zone, surface, and partition boundary meshes.

See Displaying the Mesh (p. ) for details about the items below.

You can also access the Mesh Display dialog box through the Postprocessing ribbon tab.

Postprocessing → Graphics → Mesh → New...

Controls

Mesh Name

is the name for a mesh display definition.You can specify a name or use the default name  mesh-id .

This control appears only for mesh display definitions.

Options

contains the rendering options described below.To see the effects of your selection you must click the

Display button.

Nodes

enables the display of nodes on the selected surfaces.

Edges

enables the display of mesh edges on the selected surfaces.

Faces

enables the display of mesh faces (filled meshes) on the selected surfaces.

Partitions

enables the display of partition boundaries.

Overset

Faces

Overset

when enabled, displays only the solve cells for cases with overset interfaces. Receptor cells are also

displayed if the text command define/overset-interfaces/options/render-receptor-

cells? is set to yes.

Shrink Factor

specifies the amount to shrink faces and cells. See Shrinking Faces and Cells in the Display (p. ) for

details.

Edge Type

controls the display of edges. (These items will not appear if the Edges option is turned off.)

All

enables the display of all mesh edges.

Feature

enables feature lines in an outline display. See Adding Features to an Outline Display (p. ) for details.

Outline

enables the display of the mesh outline.

Feature Angle

controls the amount of detail added to a feature outline display. See Adding Features to an Outline Dis-

play (p. ) for details. (This item will be available only if the Feature edge type is enabled.)

Surfaces

contains a list from which you can select the surfaces for which the mesh is to be drawn.

New Surface

is a drop-down list button that contains a list of surface options:

Point

opens the Point Surface Dialog Box (p. ).

Line/Rake

opens the Line/Rake Surface Dialog Box (p. ).

Plane

opens the Plane Surface Dialog Box (p. ).

Quadric

opens the Quadric Surface Dialog Box (p. ).

Iso-Surface

opens the Iso-Surface Dialog Box (p. ).

Iso-Clip

opens the Iso-Clip Dialog Box (p. ).

Structural Point

opens the Structural Point Surface Dialog Box (p. ).

Outline

selects all “outline” boundaries in the Surfaces list. If all outline boundaries are already selected, it deselects

them.

Interior

Outline

them.

Interior

selects all “interior” surfaces in the Surfaces list. If all interior surfaces are already selected, it deselects

them.

Adjacency

opens the Adjacency Dialog Box (p. ) from which you can identify and display face zones that are adja-

cent to selected cell zones.

Coloring

Automatic

nodes, edges, and faces are automatically colored by type or ID, depending on which is specified in

the Mesh Colors Dialog Box (p. ).

Colors...

opens the Mesh Colors Dialog Box (p. ).

Manual

allows you to manually specify the color of nodes, edges, and faces, if enabled under Options.

Nodes

specify the color for the nodes.

Edges

specify the color for the edges.

Faces

specify the color for the faces.

Display

displays the defined mesh plot.

Save/Display

displays the mesh in the active graphics window and saves the mesh display definition.This button appears

only for mesh display definitions and replaces the Display button.

The Set Units dialog box allows you to set the units system for any quantity used in ANSYS Fluent.

All quantities may be set to a standard system, such as SI or British, or the units of individual quantities

may be set. See Unit Systems (p. ) for details about the items below.

Controls

Quantities

displays the list of all quantities used by ANSYS Fluent for input and output.

Units

lists the units appropriate for the currently selected quantity. Selecting an item in the Units list causes

that unit to be used for the currently selected quantity.

Factor

displays the conversion factor from the currently selected units to SI.

Offset

Factor

Offset

displays the conversion offset from the currently selected units to SI.

Set All to

contains standard sets of units that are applied to all quantities when selected.

default

is similar to si, but uses degrees instead of radians for angles.

si

selects the System International (SI) standard for all units.

british

selects the English Engineering standard for all units.

cgs

selects the CGS (centimeter-gram-second) standard for all units

New...

opens the Define Unit Dialog Box (p. ), in which you can specify a customized unit for a particular

quantity.

List

displays the current units for all quantities in the console.

The Define Unit dialog box allows you to customize the units for a particular quantity. It is opened

from the Set Units Dialog Box (p. ). For details about using this dialog box, see Defining a New

Unit (p. ).

Controls

Quantity

shows the name of the quantity for which you are defining a new unit. (You cannot edit this field; the

quantity is selected in the Set Units Dialog Box (p. ).)

Unit

sets the name for the new unit.

Factor

sets the conversion factor from the currently selected units to SI.

Offset

sets the conversion offset from the currently selected units to SI.

The Mesh Colors dialog box allows you to control the colors that are used to draw meshes. It is opened

from the Mesh Display Dialog Box (p. ). See Modifying the Mesh Colors (p. ) for details about the

items below.

Controls

Options

contains options to select the method by which to set the colors.

Color by Type

Controls

Options

sets the color based on the type of zone.

Color by ID

sets the color by ID.

Types

contains a selectable list of zone types.You can select the zone type for which you want to set the color.

Colors

contains a list from which you can select a color for the selected type.

Sample

displays a sample of the currently selected color.

Reset Colors

resets the mesh colors to the default selections.

The Models task page allows you to set various generic model settings.

Models Task Page

Controls

Models

contains a listing of the various models available in ANSYS Fluent.

You can double-click an item in the Models list to open the corresponding dialog box, or you can

select the item in the list and click the Edit... button.

Multiphase

selecting this item and clicking the Edit... button opens the Multiphase Model Dialog Box (p. ).

Energy

selecting this item and clicking the Edit... button opens the Energy Dialog Box (p. ).

Viscous

selecting this item and clicking the Edit... button opens the Viscous Model Dialog Box (p. ).

Radiation

selecting this item and clicking the Edit... button opens the Radiation Model Dialog Box (p. ).

Heat Exchanger

selecting this item and clicking the Edit... button opens the Heat Exchanger Model Dialog Box (p. ).

Species

selecting this item and clicking the Edit... button opens the Species Model Dialog Box (p. ).

The following models are made available, depending on your setup of the Species dialog box.

Spark Ignition - selecting this item and clicking the Edit... button opens the Spark Ignition Dialog

Box (p. ). Note that spark ignition is only available for transient calculations.

Autoignition - selecting this item and clicking the Edit... button opens the Autoignition Model

Dialog Box (p. ). Note that autoignition is only available for transient calculations.

Inert - selecting this item and clicking the Edit... button opens the Inert Dialog Box (p. ). Note

that the inert model is only available when the non-premixed or partially premixed model is selected

in the Species Model dialog box, or when a PDF file is read.

NOx - selecting this item and clicking the Edit... button opens the NOx Model Dialog Box (p. ).

Note that the NOx model is not compatible with premixed combustion.

SOx - selecting this item and clicking the Edit... button opens the SOx Model Dialog Box (p. ).

Note that the SOx model is not compatible with premixed combustion.

Soot - selecting this item and clicking the Edit... button opens the Soot Model Dialog Box (p. ).

Note that none of the soot models are compatible with premixed combustion.

Decoupled Detailed Chemistry - selecting this item and clicking the Edit... button opens the De-

coupled Detailed Chemistry Dialog Box (p. ).

Reacting Channel Model - selecting this item and clicking the Edit... button opens the Reacting

Channel Model Dialog Box (p. ).

Discrete Phase

selecting this item and clicking the Edit... button opens the Discrete Phase Model Dialog Box (p. ).

Solidification & Melting

selecting this item and clicking the Edit... button opens the Solidification and Melting Dialog

Box (p. ).

Acoustics

Box (p. ).

Acoustics

selecting this item and clicking the Edit... button opens the Acoustics Model Dialog Box (p. ).

Structure

selecting this item and clicking the Edit... button opens the Structural Model Dialog Box (p. ).

Eulerian Wall Film

selecting this item and clicking the Edit... button opens the Eulerian Wall Film Dialog Box (p. ).

selecting this item and clicking the Edit... button opens the Potential Dialog Box (p. ).

Edit...

opens the dialog box corresponding to the selected item in the Models list.

... Multiphase Model Dialog Box

... Energy Dialog Box

...Viscous Model Dialog Box

... Radiation Model Dialog Box

...View Factors and Clustering Dialog Box

... Participating Boundary Zones Dialog Box

... Solar Calculator Dialog Box

... Heat Exchanger Model Dialog Box

... Dual Cell Heat Exchanger Dialog Box

... Set Dual Cell Heat Exchanger Dialog Box

... Heat Transfer Data Table Dialog Box

... NTU Table Dialog Box

... Copy From Dialog Box

... Ungrouped Macro Heat Exchanger Dialog Box

...Velocity Effectiveness Curve Dialog Box

... Core Porosity Model Dialog Box

... Macro Heat Exchanger Group Dialog Box

... Species Model Dialog Box

... Coal Calculator Dialog Box

... Integration Parameters Dialog Box

... Flamelet 3D Surfaces Dialog Box

... Flamelet 2D Curves Dialog Box

... Unsteady Flamelet Parameters Dialog Box

... Flamelet Fluid Zones Dialog Box

... Select Transported Scalars Dialog Box

... PDF Table Dialog Box

... Spark Ignition Dialog Box

... Set Spark Ignition Dialog Box

... Autoignition Model Dialog Box

... Inert Dialog Box

... NOx Model Dialog Box

... SOx Model Dialog Box

... Soot Model Dialog Box

... Sticking Coefficients Dialog Box

... Mechanism Dialog Box

... Reactor Network Dialog Box

... Decoupled Detailed Chemistry Dialog Box

... Reacting Channel Model Dialog Box

... Reacting Channel 2D Curves Dialog Box

... Discrete Phase Model Dialog Box

... DEM Collisions Dialog Box

... Create Collision Partner Dialog Box

... Copy Collision Partner Dialog Box

... Rename Collision Partner Dialog Box

... DEM Collision Settings Dialog Box

... Solidification and Melting Dialog Box

... Acoustics Model Dialog Box

... Acoustic Sources Dialog Box

... Acoustic Receivers Dialog Box

... Basic Shapes Dialog Box

... Interior Cell Zone Selection Dialog Box

... Structural Model Dialog Box

... Eulerian Wall Film Dialog Box

... Potential Dialog Box

The Multiphase Model dialog box allows you to set parameters for modeling multiphase flow. See

Enabling the Multiphase Model (p. ) – Including Cavitation Effects (p. ) for details.

Controls

Model

allows you to select one of four multiphase models.

Off

disables the calculation of multiphase flow.

enables the VOF model described in Volume of Fluid (VOF) Model Theory in the Theory Guide. See

Setting Up the VOF Model (p. ) for details about using the model.This is available only with the

Mixture

Mixture

enables the mixture model described in Mixture Model Theory in the Theory Guide. See Setting Up

the Mixture Model (p. ) for details about using the model.This is available only with the pressure-

Eulerian

enables the Eulerian model described in Eulerian Model Theory in the Theory Guide. See Setting Up

the Eulerian Model (p. ) for details about using the model.This is available only with the pressure-

Wet Steam

enables the wet steam model described in Wet Steam Model Theory in the Theory Guide. See Setting

Up the Wet Steam Model (p. ) for details about using the model.This is available only with the

density-based solver.

allows you to specify the number of phases for the multiphase calculation.You can specify up to

phases.

Coupled Level Set + VOF

allows you to apply an interface tracking method that couples the level set method with the VOF formu-

lation.

Volume Fraction Parameters

contains parameters related to the VOF and Eulerian model.This section of the dialog box will appear

only when Volume of Fluid or Eulerian is the selected Model.

allows you to select the desired volume tracking formulation.

Explicit

enables the Euler explicit formulation, described in The Explicit Formulation in the Theory Guide.

See Choosing Volume Fraction Formulation (p. ) for more information.

Implicit

enables the implicit formulation, described in The Implicit Formulation in the Theory Guide. See

Choosing Volume Fraction Formulation (p. ) for more information.

Volume Fraction Cutoff

Implicit

specifies a cutoff limit for the volume fraction values.The value that you provide is used as the lower

cutoff for the volume fraction. All volume fraction values in the domain below this cutoff value are

set to zero.The upper cutoff is calculated as (. - lower cutoff). All volume fraction values above the

upper cutoff value are set to ..The default value is 1e-.

Important

The Volume Fraction Cutoff value can be specified when using the Explicit formu-

lation for volume fraction.

specifies the maximum Courant number allowed near the free surface.This item will not appear if

the Implicit Scheme is selected. See Setting Time-Dependent Parameters for the Explicit Volume

Fraction Formulation (p. ) for details.

Mixture Parameters

contains options related to the Mixture model.

Slip Velocity

enables/disables the calculation of slip velocities for the secondary phases as described in Relative

(Slip) Velocity and the Drift Velocity in the Theory Guide. See also Solving a Homogeneous Multiphase

Flow (p. ).

Eulerian Parameters

contains options related to the Eulerian model.

Dense Discrete Phase Model

allows you to include the Dense Discrete Phase model (see Including the Dense Discrete Phase

Model (p. ) for details). Enabling this model automatically enables the DPM model.

Multi-Fluid VOF Model

allows you to include the multi-fluid VOF model (see Including the Multi-Fluid VOF Model (p. ) for

details).The multi-fluid VOF model allows the modeling of interface sharpening schemes and free

surface flow.

Boiling Model

allows you to include the Boiling model (see Including the Boiling Model (p. ) for details).

Boiling Model Options

allows you to select the type of boiling model to apply to your case.

RPI Boiling Model

is where the total heat flux from the wall to the liquid is partitioned into three components,

namely the convective heat flux, the quenching heat flux, and the evaporative heat flux. Details

about this model can be found in RPI Model in the Theory Guide.

Non-equilibrium Boiling

is a modification to the RPI model in order to model different boiling regimes like DNB and

critical heat flux. Details about this model can be found in Non-equilibrium Subcooled Boiling

Critical Heat Flux

is where the critical heat flux condition is characterized by a sharp reduction of local heat

transfer coefficients and the excursion of wall surface temperatures. Details about this model

can be found in Critical Heat Flux in the Theory Guide.

Number of Discrete Phase

allows you to specify the number of discrete phases when the Dense Discrete Phase Model option is

enabled.

contains an additional option for body force calculations.

enables the implicit body force treatment described in Including Body Forces (p. ).

VOF Sub-Models

contains additional sub-models that can be applied when using the VOF model.

Open Channel Flow

enables the model to study the effects of open channel flow. See Open Channel Flow in the Theory

Guide and Modeling Open Channel Flows (p. ) for details.

Open Channel Wave BC

enables the model to set specific parameters for a particular boundary for open channel wave

boundaries. See Open Channel Wave Boundary Conditions in the Theory Guide and Modeling Open

Channel Wave Boundary Conditions (p. ) for details.

Options

contains additional modeling options.

contains settings for how to model interfaces for the VOF model, Mixture multiphase model, and

Eulerian with Multi-Fluid VOF enabled. See Interface Modeling Type (p. ) for details.

Type

allows you to select the type of interface modeling to be performed.You can choose between

Sharp, Dispersed, or a hybrid Sharp/Dispersed when both types of interfaces may be present,

or when the interface is mildly sharp. See Interface Modeling Type (p. ) for more details.

enables an anti-diffusion treatment at the interface when using the Sharp interface modeling

type.This can be used to reduce the effects of numerical diffusion that may occur with coarse

meshes, high-aspect ratio cells, or large jumps in cell volume near the interface.

Interface Modeling Options...

opens the Interface Modeling Options dialog box from which you can enable Zonal Discretiz-

ation and/or Phase Localized Discretization.

Expert Options...

opens the Expert Options dialog box which contains settings for VOF time advancement when using

the Explicit formulation. Here you can set the Sub-Time Step Calculation Method and enable Solve

VOF Every Iteration. See Expert Options (p. ) for details.

The Energy dialog box allows you to set parameters related to energy or heat transfer in your model.

Controls

Energy

contains inputs related to the modeling of energy.

Energy Equation

enables/disables the calculation of energy in the model.

The Viscous Model dialog box allows you to set parameters for inviscid, laminar, and turbulent flow.

See Steps in Using a Turbulence Model (p. ) for details about using this dialog box to set up a tur-

bulent flow calculation.

Controls

Model

contains options for specifying the viscous model.

Inviscid

specifies inviscid flow.

Laminar

specifies laminar flow.

specifies turbulent flow to be calculated using the Spalart-Allmaras model. (See Spalart-Allmaras

Model in the Theory Guide for background about this model. See Setting Up the Spalart-Allmaras

Model (p. ) for details about using this model.)

k-epsilon

specifies turbulent flow to be calculated using one of three -  models. (See Standard, RNG, and

Realizable k-ε Models in the Theory Guide for background about this model. See Setting Up the k-

ε Model (p. ) for details about using this model.)

k-omega

specifies turbulent flow to be calculated using one of two -

models. (See Standard, BSL, and SST

k-ω Models in the Theory Guide for background about these models. See Setting Up the k-ω Mod-

el (p. ) for details about using this model.)

Transition k-kl-omega

specifies turbulent flow to be calculated using the Transition -

model. (See k-kl-ω Transition

Model in the Theory Guide for background about this model. See Setting Up the Transition k-kl-ω

specifies turbulent flow to be calculated using the Transition SST model. (See Transition SST Model

in the Theory Guide for background about this model. See Setting Up the Transition SST Model (p. )

for details about using this model.)

Reynolds Stress

specifies turbulent flow to be calculated using the RSM. (See Reynolds Stress Model (RSM) in the

Theory Guide for background about this model. See Setting Up the Reynolds Stress Model (p. ) for

details about using this model.)

specifies turbulent flow to be calculated using the SAS model in combination with the SST -

model. (See Scale-Adaptive Simulation (SAS) Model in the Theory Guide for background about this

model. See Setting Up Scale-Adaptive Simulation (SAS) Modeling (p. ) for details about using this

model.)

Detached Eddy Simulation

specifies turbulent flow to be calculated using the DES model. (See Detached Eddy Simulation (DES)

in the Theory Guide for background about this model. See Setting Up the Detached Eddy Simulation

Large Eddy Simulation

(3D only) specifies turbulent flow to be calculated using the LES model. (See Large Eddy Simulation

(LES) Model in the Theory Guide for background about this model. See Setting Up the Large Eddy

Simulation Model (p. ) for details about using this model.)

Spalart-Allmaras Production

contains options for the Spalart-Allmaras model.This portion of the dialog box will appear only if Spalart-

Allmaras is selected as the Model.

Vorticity-Based

selects the vorticity-based calculation of the deformation tensor  (see Equation . in the Theory

Guide).

Strain/Vorticity-Based

selects the strain/vorticity-based calculation of the deformation tensor  (see Equation . in the

Theory Guide).

k-epsilon Model

contains options for specifying which of the -  models is to be used.This portion of the dialog box will

appear only if k-epsilon is selected as the Model.

Standard

selects the standard -  model, described in Standard k-ε Model in the Theory Guide and Setting Up

the k-ε Model (p. ).

RNG

selects the RNG -  model, described in RNG k-ε Model. in the Theory Guide and Setting Up the k-

ε Model (p. ).

Realizable

selects the realizable -  model, described in Realizable k-ε Model in the Theory Guide and Setting

Up the k-ε Model (p. ).

RNG Options

specifies parameters that affect the solution of problems solved with the RNG -  model.This portion of

the dialog box will appear only if RNG is selected as the k-epsilon Model.

Differential Viscosity Model

specifies whether or not the low-Reynolds-number RNG modifications to turbulent viscosity should

be included. By default, this option is turned off. It is likely to have an effect only when the near-wall

regions in the domain are well resolved in terms of mesh density. See Differential Viscosity Modifica-

Swirl Dominated Flow

specifies whether or not the RNG modification to turbulent viscosity for swirling flows should be in-

cluded.This option is available only in 3D and 2D axisymmetric swirl solvers, and it can yield improved

predictions when solving flows with significant swirl. See Swirl Modification (p. ) for details.

k-omega Model

contains options for specifying which of the -

models is to be used.This portion of the dialog box will

appear only if k-omega is selected as the Model.

Standard

selects the standard -

model, described in Standard k-ω Model in the Theory Guide and Setting

Up the k-ω Model (p. ).

GEKO

selects the generalized -

model, described in Generalized k-ω  (GEKO) Model in the Theory Guide

and Setting up the Generalized k-ω (GEKO) Model (p. ).

BSL

selects the baseline (BSL) -

model, described in Baseline (BSL) k-ω Model in the Theory Guide and

Setting Up the k-ω Model (p. ).

SST

selects the shear-stress transport (SST) -  model, described in Shear-Stress Transport (SST) k-ω

Model in the Theory Guide and Setting Up the k-ω Model (p. ).

k-omega Options

specifies parameters that affect the solution of problems solved with the -

models.This portion of the

dialog box will appear only if k-omega is selected as the Model.

Low-Re Corrections

specifies whether corrections that improve the accuracy in predicting low Reynolds number flows

should be included.This option is available only for the -

models and the stress-omega RSM

model. See Low-Re Corrections (p. ) for details.

Shear Flow Corrections

specifies whether corrections that improve the accuracy in predicting free shear flows should be in-

cluded.This option is available only for the standard -

model and the stress-omega RSM model.

See Shear Flow Corrections (p. ) for details.

Turbulence Damping

includes the effects of turbulence damping in multiphase simulations, which is required for better

resolution of velocity gradients in the vicinity of fluid-fluid interface.When this option is enabled, you

will need to specify Damping Factor (default = ).This option is available for the VOF and Mixture

models and for the Eulerian multiphase model with the Multi-Fluid VOF model selected. See Turbu-

lence Damping (p. ) for details.

Transition SST Options

allows you to include the Roughness Correlation of rough walls as described in Transition SST and Rough

Walls in the Theory Guide.

Roughness Correlation

when enabled allows you to specify the Geometric Roughness Height as a constant value.

Reynolds-Stress Model

specifies the various Reynolds stress models (RSM).

Linear Pressure-Strain

enables the linear pressure-strain model. See Linear Pressure-Strain Model in the Theory Guide for

details.

Quadratic Pressure-Strain

enables the quadratic pressure-strain model for superior performance in a range of basic shear flows,

including plane strain, rotating plane shear, and axisymmetric expansion/contraction. See Quadratic

Pressure-Strain Model in the Theory Guide for details. Note that this option cannot be used with the

Wall Reflection Effects option or the Enhanced Wall Treatment.

Stress-Omega

enables a stress-transport model that is based on the omega equations and LRR model [] (p. ).

This model is ideal for modeling flows over curved surfaces and swirling flows. See Stress-Omega

Model in the Theory Guide for details.

Stress-BSL

enables a linear model for the pressure-strain term like the Stress-Omega model, but solves the scale

equation from the baseline (BSL) -

model, and thus removes the free-stream sensitivity observed

with the Stress-Omega model. Like the Stress-Omega model, it is recommended for modeling flows

over curved surfaces and swirling flows. See Stress-BSL Model in the Theory Guide for details.

Reynolds-Stress Options

specifies parameters that affect the solution of problems solved with the Reynolds stress model.This

portion of the dialog box will appear only if Reynolds Stress is selected as the Model.

Wall BC from k Equation

enables the explicit setting of boundary conditions for the Reynolds stresses near the walls, using the

values computed with Equation . in the Theory Guide. See Solving the k Equation to Obtain Wall

Boundary Conditions (p. ) for details.This option is on by default.

Wall Reflection Effects

enables the calculation of the component of the pressure strain term responsible for the redistribution

of normal stresses near the wall. See Including the Wall Reflection Term (p. ) for details. Note that

this option is not available if you have enabled the Quadratic Pressure-Strain Model.

RANS Model

contains options for the subgrid-scale model used by the Detached Eddy Simulation Model.This portion

RANS Model

of the dialog box will appear only if Detached Eddy Simulation Model is selected as the Model.

enables the Spalart-Allmaras RANS model. See Detached Eddy Simulation (DES) in the Theory Guide for

details.

Realizable k-epsilon

enables the Realizable -  RANS model. See Detached Eddy Simulation (DES) in the Theory Guide for

details.

SST k-omega

enables the SST -

RANS Model. See Detached Eddy Simulation (DES) in the Theory Guide for details.

DES Options

contain the option to include a delayed Detached Eddy Simulation.

Delayed DES

is useful for RANS meshes with high aspect ratios in the boundary layer.This option preserves the

RANS model throughout the boundary layer. (See Delayed Detached Eddy Simulation (DDES) (p. )

for details.)

Subgrid-Scale Model

contains options for the subgrid-scale model used by the LES model.This portion of the dialog box will

appear only if Large Eddy Simulation is selected as the Model.

selects the Smagorinsky-Lilly subgrid-scale model described in Subgrid-Scale Models in the Theory

Guide.

WALE

selects the Wall-Adapting local Eddy-Viscosity model described in Wall-Adapting Local Eddy-Viscosity

(WALE) Model in the Theory Guide.

WMLES

selects the algebraic Wall-Modeled LES model described in Algebraic Wall-Modeled LES Model (WMLES)

selects the algebraic Wall-Modeled LES -  model described in Algebraic WMLES S-Omega Model

selects the dynamic kinetic energy subgrid-scale model described in Dynamic Kinetic Energy Subgrid-

Scale Model in the Theory Guide.

LES Model Options

contains options for the Large Eddy Simulation model.This portion of the dialog box will appear only if

Large Eddy Simulation is selected as the Model.

enables the dynamic stress model. It is available for selection when the Smagorinsky-Lilly is selected,

and is enabled (and cannot be disabled) when the Kinetic-Energy Transport is selected.

Dynamic Energy Flux

enables the dynamic energy flux model. It is available when the LES model option Dynamic Stress

Dynamic Scalar Flux

enables the dynamic computation of turbulent Sc (

in Equation . in the Theory Guide). See

Definition of the Mixture Fraction in the Theory Guide for details. It is available when the LES model

option Dynamic Stress is enabled.

Dynamic Fvar

enables the dynamic mixture fraction variance model. It is available when Non-Premixed Combustion

or Partially Premixed Combustion is selected in the Species Model Dialog Box (p. ). See The Non-

Premixed Model for LES in the Theory Guide for details.

Near-Wall Treatment

specifies the near-wall treatment to be used for modeling turbulence. See Near-Wall Treatments for Wall-

Bounded Turbulent Flows in the Theory Guide for details about the available methods.This portion of

the dialog box will appear if k-epsilon or Reynolds Stress is selected as the Model.

enables the use of standard wall functions (described in Standard Wall Functions in the Theory Guide).

enables the use of scalable wall functions (described in Scalable Wall Functions in the Theory Guide).

enables the use of non-equilibrium wall functions (described in Non-Equilibrium Wall Functions in

enables the use of the enhanced wall treatment (described in Enhanced Wall Treatment ε-Equation

(EWT-ε) in the Theory Guide). Note that this option will not appear if you have enabled the Quadratic

Pressure-Strain Model under Reynolds-Stress Options.

enables the use of the Menter-Lechner near-wall treatment (described in Menter-Lechner ε-Equation

(ML-ε) in the Theory Guide). Note that this option is only available when k-epsilon is selected for the

Model.

enables you to hook a user-defined function, used to define the Law of the Wall. See User-Defined

Wall Functions in the Theory Guide for more information.

Enhanced Wall Treatment Options

allows you to include pressure gradient or thermal effects in the calculation. See Near-Wall Treatments

for Wall-Bounded Turbulent Flows in the Theory Guide.

Pressure Gradient Effects

enables the effect of pressure gradient.

Thermal Effects

enables thermal effects in the calculation.This option appears only if the energy equation is enabled.

Options

contains general options for viscous modeling.

Viscous Heating

(if enabled) includes the viscous dissipation terms in the energy equation.This option is recommended

when you are solving a compressible flow. Note that this option is always turned on when one of the

density-based solvers is used; you will not be able to turn it off.

Low-Pressure Boundary Slip

includes slip boundary conditions for velocity and temperature for modeling fluid flow at very low

pressures as in semiconductor fabrication devices. See Slip Boundary Formulation for Low-Pressure

Gas Systems in the Theory Guide.This option is available only for laminar flows.

Full Buoyancy Effects

enables the inclusion of buoyancy effects on . See Including Turbulence Generation Due to Buoy-

ancy (p. ) for details.This option will appear if k-epsilon or Reynolds Stress is selected as the

Model and a nonzero gravitational acceleration has been specified in the Operating Conditions Dialog

Box (p. ).

Curvature Correction

when enabled, modifies the turbulence production term to sensitize the standard eddy-viscosity

models to the effects of streamline curvature and system rotation.This is available for the Spalart-

Allmaras, k-epsilon, k-omega, Transition SST, Scale-Adaptive Simulation, and Detached Eddy

Simulation with the SST k-omega model.

Curvature Correction Options

CCURV

specifies a coefficient used in the curvature correction term to influence the strength of the

curvature correction if needed for a specific flow. Can be a constant or specified via UDF.

when enabled, can improve the prediction of free shear layers at high Mach numbers.This is available

when the compressible form of the ideal gas law or the real-gas model is activated for k-epsilon, k-

omega, Transition k-kl-omega, Reynolds Stress, Scale-Adaptive Simulation, and Detached Eddy

Simulation with the Realizable k-epsilon model. For details, see Model Enhancements (p. ).

Mixture Drift Force

includes the effect of turbulent drift velocity when using the Mixture model. See Modeling Turbu-

lence (p. ). Note that this option is only available when using the Mixture model with Slip Velocity

enabled in the Multiphase Model dialog box. See Including Mixture Drift Force (p. ).

when enabled, the Kato-Launder modification for the production term limits the production term in

the turbulence equation. For details see, Production Limiters for Two-Equation Models in the Fluent

when enabled, limits the production term in the turbulence equation. For details, see Production

Limiters for Two-Equation Models in the Fluent Theory Guide.

Intermittency Transition Model

enables the Intermittency Transition model to account for transitional effects.This option is only

available for the BSL -

, SST -

, Scale-Adaptive Simulation with BSL / SST, and Detached Eddy

Simulation with BSL / SST models. For details, see Intermittency Transition Model in the Theory Guide.

Intermittency Transition Options

contains an option for the Intermittency Transition model.This group box is only available when the In-

termittency Transition Model option is enabled.

Include Crossflow Transition

includes the effects of crossflow instability. For details, see Transport Equations for the Intermittency

Transition Model in the Theory Guide.

Turbulence Multiphase Model

contains options for multiphase turbulence models.This portion of the dialog box will appear if Eulerian

is selected as the Model in the Multiphase Model Dialog Box (p. ).

Mixture

specifies the (default) mixture turbulence model.

Dispersed

specifies the dispersed turbulence model.

Per Phase

specifies the calculation of a set of turbulence equations for each phase.

See Turbulence Models in the Theory Guide for details about the available multiphase turbulence

models.

GEKO Options

contains options for the GEKO model.

Wall Distance Free

Selects the wall distance free version of the GEKO model.

CSEP

Specifies

parameter to optimize flow separation from smooth surfaces.

CNW

Specifies

parameter to optimize flow in non-equilibrium near wall regions (such as heat transfer

or

).

CMIX

Specifies

parameter to optimize strength of mixing in free shear flows.

CJET

Specifies

parameter to optimize free shear layer mixing (optimize free jets independent of

mixing layer).

Blending Function

Specifies the blending function,

, which deactivates these parameters inside boundary layers.

See Generalized k-ω  (GEKO) Model in the Fluent Theory Guide for details about the GEKO model

options.

Model Constants

contains constants used in the equations for turbulence. See Spalart-Allmaras Model, Standard k-ε Model,

RNG k-ε Model, k-kl-ω Transition Model, Transition SST Model, Realizable k-ε Model, Reynolds Stress

Model (RSM), Standard k-ω Model, Shear-Stress Transport (SST) k-ω Model, and Large Eddy Simulation

(LES) Model in the Theory Guide for details about these constants.

Cb1

(only for the Spalart-Allmaras model) is the constant

Cb2

Cv1

Cw2

Cw3

Cprod

(only for the Spalart-Allmaras model when the Strain/Vorticity-Based Production option is used) is

Cmu

(only for the standard or RNG -  model, the RSM, or the -

Transition model) is the constant

that is used to compute

.

C1-Epsilon

(only for the standard or RNG -  model or the RSM) is the constant

used in the transport equation

for .

C2-Epsilon

(only for the standard, RNG, or realizable -  model or the RSM) is the constant

used in the

transport equation for .

C3-Epsilon

(only for the dispersed or per-phase -  multiphase models) is the constant

C-lambda

(only for the -

in the definition of the effective length,

CR

used in the definition of , where  represents

the averaged effect of the breakdown of streamwise fluctuations into turbulence during bypass

ANAT

ATS

CNAT, crit

ANAT

ATS

CNAT, crit

CTS, crit

CRNAT

Anu

CINT

Cw1

Cw3

Calpha-teta

Ctaul

SDR Prandtl Number

(only for the standard -

model and the -

Transition model) is the effective “Prandtl” number

for the transport of the specific dissipation rate,

.

Ca1

(only for the Transition SST model)

Ca2

Ce1

Ce2

C_thetat

C_s1

Intermit. Prandtl #)

Re_theta. Prandtl #)

C Shielded DES

(only for the SDES or SBES model) is a constant that serves the same purpose as

in the DDES tur-

bulence model (see Equation . in the Theory Guide).

Csdes

(only for the SDES or SBES model) is

, as described in Shielded Detached Eddy Simulation (SDES)

Cwale

(only for the WALE subgrid-scale model of the LES or SBES model) is

, as described in Wall-Adapting

Local Eddy-Viscosity (WALE) Model in the Theory Guide.

CREAL (GEKO)

(only for the GEKO model) is

, as described in Generalized k-ω  (GEKO) Model in the Fluent Theory

Guide.

CNW_SUB (GEKO)

, as described in Generalized k-ω  (GEKO) Model in the Fluent

CJET_AUX (GEKO)

CBF_TUR (GEKO)

CBF_LAM (GEKO)

Swirl Factor

in Equation . in the Theory Guide.This item appears for the RNG -  model

when the Swirl Dominated Flow option is turned on.

Alpha*_inf

(only for the standard, BSL, or SST -

model, and the Transition SST model) is the constant

in

Alpha_inf

in

Alpha_0

model with the Low-Re Corrections option enabled) is the

constant

Beta*_inf

in

Beta_i

model) is the constant

R_beta

R_k

constant

R_k

constant

R_w

constant

Zeta*

model when the Compressibility Effects option is enabled)

Mt0

a1

(only for the SST -

Beta_i (Inner)

(only for the BSL or SST -

in Model Con-

stants in the Theory Guide.

Beta_i (Outer)

Cs

is a constant that depends on the turbulence model. For LES, it is the Smagorinsky constant

in

Equation . in the Theory Guide. For SAS, it is the high wave number damping coefficient

in

C1-PS

(only for RSM) is the constant

C2-PS

C1’-PS

C2’-PS

C1-SSG-PS

(only for RSM with the Quadratic Pressure-Strain Model) is the constant

C1’-SSG-PS

C1-SSG-PS

C2-SSG-PS

C3-SSG-PS

C3’-SSG-PS

C4-SSG-PS

C5-SSG-PS

Prandtl Number

TKE Prandtl Number

(only for the standard or realizable -  model, the standard -

model, the -

Transition model,

or the RSM) is the effective “Prandtl” number for transport of turbulence kinetic energy

.This effective

Prandtl number defines the ratio of the momentum diffusivity to the diffusivity of turbulence kinetic

energy via turbulent transport.

TKE (Inner) Prandtl #

model, and the Transition SST model) is the effective “Prandtl” number

for the transport of turbulence kinetic energy,

, inside the near-wall region. See Modeling the

Turbulent Viscosity in the Theory Guide for details.

TKE (Outer) Prandtl #

, outside the near-wall region. See Modeling the

TDR Prandtl Number

is the effective “Prandtl” number for transport of the turbulent dissipation rate,

, for the standard

or realizable -  model or the RSM.This effective Prandtl number defines the ratio of the momentum

diffusivity to the diffusivity of turbulence dissipation via turbulent transport.

SDR (Inner) Prandtl #

SDR (Outer) Prandtl #

Dispersion Prandtl Number

(only for the -  multiphase models) is the effective “Prandtl” number for the dispersed phase,

.

See Turbulence Models in the Theory Guide for details.

Energy Prandtl Number

(for any turbulence model except the RNG -  model) is the turbulent Prandtl number for energy,

, in Equation . in the Theory Guide. (This item will not appear for the LES model if the Dynamic

Energy Flux option has been enabled, or for premixed or partially premixed combustion models.)

For non-premixed and partially premixed combustion, the energy Prandtl Number is set equal to the

PDF Schmidt Number.

Wall Prandtl Number

(for all turbulence models) is the turbulent Prandtl number at the wall,

Theory Guide. (This item will not appear for adiabatic premixed combustion or partially premixed

combustion models.)

Turbulent Schmidt Number

(for turbulent species transport calculations using any turbulence model except the RNG -  model)

is the turbulent Schmidt number,

, in Equation . in the Theory Guide. (This item will not appear

for the LES model if the Dynamic Scalar Flux option has been enabled.)

PDF Schmidt Number

(for non-premixed or partially premixed combustion calculations using any turbulence model) is the

model constant

Production Limiter Clip Factor

This coefficient is used by the Production Limiter. For details, see Equation . in the Fluent Theory

Guide.

User-Defined Transition Correlations

(only for the Transition SST model) allows you to select the user-defined correlations for F_length,

Re_thetac, Re_thetat.

User-Defined Functions

allows you to select the user-defined functions for various constants.

appears for Spalart Allmaras,

,

, DES, SDES with BSL / SST models, and SBES with BSL / SST.

You can select the user-defined functions for turbulent viscosity in the drop-down list.

Prandtl Numbers, Prandtl and Schmidt Numbers

contains a list of relevant Prandtl and Schmidt numbers for which you can select user-defined functions.

allows you to select a user-defined function to define the TKE Prandtl number for the standard

and realizable -  models and the standard -

model.

allows you to select a user-defined function to define the TDR Prandtl number for the standard

and realizable -  models.

allows you to select a user-defined function to define the turbulent Prandtl number for energy,

when energy is enabled for all turbulence models except the RNG -  model. (This item will not

appear for the LES model if the Dynamic Energy Flux option has been enabled.)

allows you to select a user-defined function to define the turbulent Prandtl number at the wall

for all turbulence models when energy is enabled.

allows you to select a user-defined function to define the turbulent Schmidt number when species

transport is enabled for all turbulence models except the RNG -  model. (This item will not appear

allows you to select a user-defined function to define the SDR Prandtl number for the standard

model.

Subgrid-Scale Turbulent Viscosity

allows you to select a user-defined function for the subgrid-scale turbulent viscosity for the LES

model.

Scale-Resolving Simulation Options

allows you to combine two turbulence models, which are applied on the appropriate regions of the flow

domain. For additional information, see Scale-Resolving Simulation (SRS) Models (p. ).

allows you to apply SAS in combination with the following

based URANS models: the Standard or

BSL -

based Reynolds stress models. For additional

information, see Setting Up Scale-Adaptive Simulation (SAS) Modeling (p. ).

Detached Eddy Simulation (DES)

allows you to apply DES in combination with the BSL -

model and Transition SST model. For addi-

tional information, see Detached Eddy Simulation (DES) (p. ).

Stress Blending (SBES) / Shielded DES

allows you to apply SBES or SDES in combination with the BSL -

model, and

Transition SST model. See Stress-Blended Eddy Simulation (SBES) and Shielded Detached Eddy Simu-

lation (SDES) in the Theory Guide for details.

Shielding Functions

allows you to select the shielding functions (SST F1 Function, SST F2 Function, DDES, and IDDES) for

the Detached Eddy Simulation model with the BSL -

model, and Transition SST model.

(see Shielding Functions for the BSL / SST / Transition SST Detached Eddy Simulation Model (p. ) for

details).

SBES / SDES Options

allows you to define the following settings as part of the SBES or SDES model:

Hybrid Model

specifies that the hybrid RANS-LES model used is either SDES (Shielded DES model), SBES (Stress-

Blended Eddy Simulation model), or SBES with User-Defined Function. See Including the SDES or

SBES Model with BSL, SST, and Transition SST Models (p. ) for details.

contains options for the subgrid-scale model used in the LES region of your Stress-Blended Eddy

Simulation.This portion of the dialog box will appear only if SBES or SBES with User-Defined

Function is selected as the Hybrid Model.

Guide.

Dynamic Smagorinsky

selects the Smagorinsky-Lilly subgrid-scale model (described in Subgrid-Scale Models in the

Theory Guide) with the dynamic stress model enabled.

WALE

selects the Wall-Adapting local Eddy-Viscosity model described in Wall-Adapting Local Eddy-Vis-

cosity (WALE) Model in the Theory Guide.

selects the algebraic Wall-Modeled LES -  model described in Algebraic WMLES S-Omega

Model Formulation in the Theory Guide.

Update Interval k-omega

Sets the number of time steps between updates of the -

part of the SBES model.

The Radiation Model dialog box allows you to select a model for radiation heat transfer and set the

associated parameters. See Using the Radiation Models (p. ) – Defining Non-Gray Radiation for the

DO Model (p. ) for details about the items below.

Controls

Model

indicates which model, if any, is used to calculate radiation heat transfer. See Modeling Radiation (p. )

for details about modeling radiation heat transfer.

Off

disables the calculation of radiation heat transfer.

Rosseland

enables the Rosseland radiation model.

P1

enables the P- radiation model.

Discrete Transfer (DTRM)

enables the discrete transfer radiation model (DTRM).

Surface to Surface (S2S)

enables the surface-to-surface (S2S) radiation model.

Discrete Ordinates (DO)

enables the discrete ordinates (DO) radiation model.

Monte Carlo (MC)

enables the Monte Carlo (MC) radiation model.

DO/Energy Coupling

allows you to couple the energy and DO intensity equations at each cell, solving them simultaneously.

See Defining Non-Gray Radiation for the DO Model (p. ) for details.

Iteration Parameters

contains parameters related to the DTRM, S2S, and the DO models.This portion of the dialog box will

appear only if Discrete Transfer (DTRM), Surface to Surface (S2S), or Discrete Ordinates (DO) is selected

as the Model.

Energy Iterations per Radiation Iteration

controls the frequency with which the radiation terms are updated as the continuous phase solution

proceeds.The Energy Iterations per Radiation Iteration parameter is set to  by default.This implies

that the radiation calculation is performed once every  iterations of the solution process. Increasing

the number can speed the calculation process, but may slow overall convergence.

Maximum Number of Radiation Iterations

controls the maximum number of iterations of the radiation calculation during each global iteration.

The default setting of  means that the radiosity will be updated up to  times.The actual number of

iterations will be less if the residual convergence criterion is exceeded at any point during these iter-

ations.

This item appears only when Discrete Transfer or Surface to Surface is selected as the

Model.

Residual Convergence Criteria

determines when the radiation intensity update is converged. It is defined as the maximum normalized

Model.

change in the surface intensity from one radiation iteration to the next (see Equation . (p. )).

Model.

Target Number of Histories

determines the number of photon histories to be tracked for the Monte Carlo simulation.Too small

of a number will produce "speckled" results. Increasing the target number of histories produces a

smoother and more accurate solution, but at the expense of higher computation effort.

This item appears only when Monte Carlo is selected.

View Factors and Clustering

contains parameters related to the S2S model.This portion of the dialog box will appear only if Surface

to Surface is selected as the Model. See Setting Up the S2S Model (p. ) for more information about

the use of these parameters.

Settings...

opens the View Factors and Clustering Dialog Box (p. ), in which you can set parameters related

to surface clusters and view factors.

Compute/Write/Read...

allows you to compute the view factors, write the computed view factors to a file, and read the file

into ANSYS Fluent.When you click Compute/Write/Read..., The Select File Dialog Box (p. ) will

open so that you can specify a name for the file where ANSYS Fluent should save the view factors

after computing them, and indicate whether the files should be saved in binary format.

Read Existing File...

opens The Select File Dialog Box (p. ), in which you can specify the file from which ANSYS Flu-

ent should read view factors.

Angular Discretization

contains parameters for angular discretization and pixelation for the DO model.This portion of the dialog

box will appear only if Discrete Ordinates is selected as the Model. See Setting Up the DO Model (p. )

for more information about the use of these parameters.

Theta Divisions, Phi Divisions

define the number of control angles used to discretize each octant of the angular space (see Fig-

ure . : Angular Coordinate System in the Theory Guide).

Theta Pixels, Phi Pixels

are used to control the pixelation that accounts for any control volume overhang (see Figure . : Pixela-

tion of Control Angle in the Theory Guide and the figures and discussion preceding it).

Radiation Mesh Options

This portion of the dialog box will appear only if the Monte Carlo model is selected.

Target Cells Per Volume Cluster

Coarsens the radiation mesh used by the MC model. See Setting Up the MC Model (p. ) for more

information about the use of this parameter.

Non-Gray Model

contains parameters related to the non-gray P-, DO, or MC model.This portion of the dialog box will

appear only if P1, Discrete Ordinates, or Monte Carlo is selected as the Model. See Setting Up the P-

Model with Non-Gray Radiation (p. ), Defining Non-Gray Radiation for the DO Model (p. ), or Setting

Up the MC Model (p. ) for more information about the use of these parameters.

Number of Bands

specifies the number of bands for the non-gray radiation.

Wavelength Intervals (n=)

contains inputs that define each wavelength band. (It appears only when the Number of Bands is

nonzero.) For each band, you can specify a Name, as well as the Start and End wavelength of the

band in m. Note that the wavelength bands are specified for vacuum (

). ANSYS Fluent will

automatically account for the refractive index in setting band limits for media with  different from

unity.

Solar Load

contains parameters related to solar load model that can be used to calculate radiation effects from the

sun’s rays that enter a computational domain. It is available only for the 3D version of ANSYS Fluent. See

Solar Load Model (p. ) for more information about the use of these parameters.

Model

indicates which model is used to calculate radiation effects.

Off

disables the calculation of solar radiations.

Solar Ray Tracing

enables the solar ray tracing algorithm

DO Irradiation

enables the DO irradiation option. Select Discrete Ordinates under Model before selecting this

option.

Solar Calculator

opens the Solar Calculator Dialog Box (p. ).

Sun Direction Vector

contains the components of sun direction vector.

X,Y, Z

are the components of the sun direction vector.

Use Direction Computed from Solar Calculator

enables the use of direction vector computed from the solar calculator.

Illumination Parameters

contains illumination options.

Direct Solar Irradiation

is the amount of energy per unit area due to direct solar irradiation.

Diffuse Solar Irradiation

is the amount of energy per unit area due to diffuse solar irradiation.

Spectral Fraction

is the fraction of incident solar radiation in the visible part of the solar radiation spectrum.The spectral

fraction is not used for DO irradiation since the DO implementation is intended only for a single band.

This parameter is available only for Solar Ray Tracing.

Update Parameters

contains update parameters for transient simulations.

Time Steps per Solar Load Update

specifies the number of time steps that will direct the ANSYS Fluent solver to update the solar load

The View Factors and Clustering dialog box allows you to set parameters related to surface clusters

and view factors for the surface-to-surface radiation model. See Setting Up the S2S Model (p. ) for

information about using this dialog box.

Controls

Clustering

contains the methods and settings for creating surface clusters. See Forming Surface Clusters (p. ) for

information about surface cluster settings.

Options

gives you a choice of forming clusters either manually or automatically.

Manual

allows you to form clusters manually.

Automatic

allows ANSYS Fluent to form the cluster automatically.

Manual

(available only when the Manual option is enabled) allows you to set the faces per surface cluster

(FPSC) value for walls and inlet and outlet boundaries.

Faces per Surface Cluster for Flow Boundary Zones

specifies the number of faces in each surface cluster for inlet and outlet boundaries (that

is, exhaust fan, inlet vent, intake fan, outlet vent, mass-flow inlet, mass-flow outlet, pressure

far-field, pressure inlet, pressure outlet, outflow, and velocity inlet boundaries). This FPSC

value can also be applied to all walls that are adjacent to fluid zones by clicking the Apply

to All Walls button. The default is set to . See Clustering in the Theory Guide for details

Apply to All Walls

applies the value specified in the Faces per Surface Cluster for Flow Boundary Zones field to

all walls that are adjacent to fluid zones.

Automatic

(available only when the Automatic option is enabled) allows you to assign different faces per surface

cluster (FPSC) values to the walls automatically, based on the distance of the walls from and the FPSC

values of the walls that are defined as critical.

Maximum Faces per Surface Cluster

specifies the maximum number of faces per surface cluster automatically assigned to non-critical

wall zones adjacent to fluid zones.The default is set to .

Compute

results in ANSYS Fluent automatically calculating and updating the face per surface cluster values

in the boundary conditions dialog box for non-critical wall zones adjacent to fluid zones, without

computing the clusters.

View Factors

contains settings for computing the view factors. See Setting Up the View Factor Calculation (p. ) for

information about view factor calculation settings.

Basis

specifies how surfaces are defined for the calculation of view factors. See Selecting the Basis for

Computing View Factors (p. ) for more information.

Face to Face

Basis

specifies that the surfaces used to calculate the view factors are the boundary faces.

Cluster to Cluster

specifies that the surfaces used to calculate the view factors are the clusters defined by the settings

in the Clustering group box.The cluster to cluster basis is only available for 3D cases.

Surfaces

specifies the geometric orientation of surface pairs with respect to each other when using the hemicube

method.

Blocking

specifies that the view factor calculation accounts for surfaces that block the views between the

surfaces under consideration.

Nonblocking

specifies that the view factor calculation does not account for surfaces that block the views

between the surfaces under consideration.

Method

specifies the method for computing the view factors. See Selecting the Method for Computing View

Factors (p. ) for information about choosing a method.

Hemicube

specifies the use of the hemicube method for computing the view factors.The hemicube method

is available only for 3D and axisymmetric cases, and should not be used if any of the zones are

defined as periodic or symmetry boundaries.

Ray Tracing

specifies the use of the ray tracing method for computing the view factors. For 2D cases, the

number of rays used with this method is two times the value set for Resolution in the Parameters

group box; for 3D cases, the number of rays is three times the square of the Resolution value.

contains settings related to the hemicube and ray tracing methods for computing the view factors.

All of these inputs are available when Hemicube is selected under Method, whereas only Resolution

is available when Ray Tracing is selected. See Selecting the Method for Computing View Factors (p. )

for information about setting the method parameters.

Resolution

specifies the resolution of the hemicube.The default value is set to .You can increase the value

to reduce aliasing effects that can lead to overestimated or underestimated view factors.

Subdivisions

specifies the number of subfaces into which each face is divided.The default value is set to .

This parameter is only available when the hemicube method is used in conjunction with the face

to face basis.

Normalized Separation Distance

specifies the ratio of the minimum face separation to the effective diameter of the face.The default

value is set to .This parameter is only available for the hemicube method.

Zones Participating in View Factor Calculation

allows you to define which boundary zones participate in the view factor calculation. See Specifying

Select...

opens the Participating Boundary Zones Dialog Box (p. ), where you can define which boundary

zones participate in the view factor calculation.

The Participating Boundary Zones dialog box allows you to define which boundary zones participate

in the view factor calculation, to display zones in the graphics window, and set the temperature of

zones that do not participate in the view factor calculation. See Specifying Boundary Zone Participa-

tion (p. ) for details. This dialog box opens when you click the Select... button next to the Zones

Participating in View Factor Calculation label in the View Factors and Clustering dialog box.

Controls

Maximum Distance from Critical Zone

allows you to view the maximum distance between critical zones and other zones, and set all boundary

zones that are located beyond a certain distance from a critical zone as not participating in the view factor

To All Other Zones

displays the maximum of the distances between the centroids of critical and all other wall, inlet, and

exit zones when the Compute button is clicked.This field is not editable.This is only available when

using the Automatic option for clustering.

Compute

calculates the distances between the centroids of critical zones and all the other wall, inlet, and exit

zones and displays the maximum value in the To All Other Zones field and the To Participating

Zones text-entry box. It requires the definition of the critical zone.

To Participating Zones

exit zones when the Compute button is clicked. Unlike the To All Other Zones field, you can edit

this text-entry box.You can specify the maximum distance allowed between the centroids of critical

zones and all other wall, inlet, or exit zones that participate in the view factor calculation; when you

click the Apply button, all of the zones will be marked as either participating or not participating,

according to the distance criteria you specified. Note that this field is only available when using the

Automatic option for clustering.

Apply

marks all of the wall, inlet, and exit zones as either participating or not participating in the view factor

calculation, depending on whether the distance from their centroid to the centroid of a critical zone

is equal to or less than value entered for To Participating Zones.The Participating Boundary Zones

and Non-Participating Boundary Zones lists will be updated accordingly.

Participating Boundary Zones

shows all the zones that are participating in the view factor calculation.You can select a zone and click

the arrow button that points to the right to move the zone to the Non-Participating Boundary Zones

list.

Non-Participating Boundary Zones

shows all the zones that are not participating in the view factor calculation.You can select a zone and

click the arrow button that points to the left to move the zone to the Participating Boundary Zones list.

Display Zones

displays any zones selected in the Participating Boundary Zones and Non-Participating Boundary

Zones lists in the graphics window.

Non-Participating Boundary Zones Temperature

allows you to specify the temperature of the zones that do not participate in the view factor calculation.

The Solar Calculator dialog box allows you to set parameters related to the calculation of solar load

models. See Solar Load Model (p. ) for details. This dialog box opens when you click the Solar Cal-

culator... button in the Radiation Model dialog box.

Controls

Global Position

contains the parameters to define the position of solar radiation.

Longitude

Controls

Longitude

specifies the longitude of the desired location in degrees.Values may range from

to

, where

negative values indicate the Western hemisphere and positive values indicate the Eastern hemisphere.

Latitude

specifies the latitude of the desired location in degrees.Values may range from

(South pole) to

(North pole) with  defined as the equator.

Timezone

specifies the local time zone of the desired location in hours relative to Greenwich Mean Time (+-

GMT).This integer value can range from

to

.

Starting Date and Time

contains parameters to specify date and time.

Day of Year

contains parameters to specify day and month.

Time of Day

contains parameters to specify hour and minutes.

Mesh Orientation

specifies the orientation as the vectors for North and East in the CFD grid system of coordinates.

Solar Irradiation Method

contains parameters to choose the solar irradiation method.

Theoretical Maximum

enables theoretically maximum solar irradiation method.

Fair Weather Conditions

enables fair weather condition solar irradiation method.

Sunshine Factor

is a linear reduction factor for the computed incident load that allows for cloud cover to be accounted

for, if appropriate.

The Heat Exchanger Model dialog box allows you to define a heat exchanger as part of your model.

See Modeling Heat Exchangers (p. ) for details about using the items below.

Controls

Options

contains options related to the heat exchanger model. See Choosing a Heat Exchanger Model (p. ) for

Controls

Options

details about the differences between the models associated with these options.

Dual Cell Model

allows you to enable or disable the Dual Cell heat exchanger model.When this option is enabled, the

corresponding Define... button opens the Dual Cell Heat Exchanger Dialog Box (p. ).

Ungrouped Macro Model

allows you to enable or disable the Ungrouped Macro heat exchanger model.When this option is

enabled, the corresponding Define... button opens the Ungrouped Macro Heat Exchanger Dialog

Box (p. ).

Macro Model Group

allows you to enable or disable the Macro heat exchanger group model.When this option is enabled,

the corresponding Define... button opens the Macro Heat Exchanger Group Dialog Box (p. ).

The Dual Cell Heat Exchanger dialog box allows you to use the NTU method for heat transfer calcu-

lations. This model allows the solution of auxiliary flow on a separate mesh (other than the primary

fluid mesh). See Using the Dual Cell Heat Exchanger Model (p. ) for information about using this

Controls

contains a list of predefined heat exchangers.

New...

opens the Set Dual Cell Heat Exchanger Dialog Box (p. ).

Copy

opens the Copy From Dialog Box (p. ), which allows you to copy the currently selected heat exchanger.

Delete

removes the currently selected heat exchanger.

Modify...

The Set Dual Cell Heat Exchanger dialog box allows you to define the heat exchanger parameters.

See Using the Dual Cell Heat Exchanger Model (p. ) for details about using this dialog box.

Controls

Name

allows you to specify a name for the dual cell heat exchanger.

Fluid Zones

allows you to specify the fluid zone parameters for the heat exchanger.

Number of Passes

specifies the number of passes for the heat exchanger.

Primary Fluid Zone

allows you to specify the fluid of the primary fluid zone for the heat exchanger.

Auxiliary Fluid Zone

allows you to specify the fluid for the auxiliary fluid zone, per pass.

Important

Heat Rejection

contains parameters specific to the rejection of heat in the heat exchanger.

Options

allows you to specify how the heat rejection in the heat exchanger is computed.

Fixed Heat Rejection

allows you to specify heat rejection parameters.

Fixed Inlet Temperature

allows you to use total heat rejection as the desired output.

Heat Rejection Targeted

allows you to specify the heat rejection desired from the heat exchanger (available only when the

Fixed Heat Rejection option is enabled).

Inlet Zone for Temperature Updates

allows ANSYS Fluent to change the temperature of the specified inlet zone in order to match the

targeted heat rejection (available only when the Fixed Heat Rejection option is enabled).

Temperature Update Under-Relaxation

controls convergence (available only when the Fixed Heat Rejection option is enabled).

Iteration Interval Between Temperature Updates

controls divergence (available only when the Fixed Heat Rejection option is enabled).

Performance Data

contains parameters for specifying the heat exchanger’s performance data.

Options

allows you to choose between using raw performance data or NTU performance data.

Raw Data

allows you to specify raw performance data for the heat exchanger.

NTU Data

allows you to specify NTU performance data for the heat exchanger.

Heat Exchanger Performance Data

contains parameters concerning the heat exchanger’s performance data.

NTU Table

opens the NTU Table Dialog Box (p. ) (available only when the NTU Data option is enabled).

Heat Transfer Table

opens the Heat Transfer Data Table Dialog Box (p. ) (available only when the Raw Data option

is enabled).

Effectiveness-NTU Relation

computes the NTU values from the heat transfer data. Choose cross-flow-unmixed, parallel-

flow, or counter-flow, all of which are described in NTU Relations (available only when the Raw

Data option is enabled).

Reference Inlet Temperature

allows you to specify the inlet reference temperature for the primary and the auxiliary fluids.

(Available only when the Raw Data option is enabled.)

Frontal Area

allows you to specify the frontal area for the heat exchanger.

Primary Fluid

allows you to specify a value for the Core Frontal Area for the primary fluid, or to compute the value

from a surface zone using the Compute From drop-down list.

Auxiliary Fluid

allows you to specify a value for the Core Frontal Area for the auxiliary fluid, or to compute the value

Coupling

specifies parameters when you want to couple the heat exchanger passes.

specifies, by default, the mass-weighted average for the temperature of the outlet of Pass  to the

inlet of Pass . Similarly, the mass-weighted-average temperature of the outlet of Pass  will be applied

at the inlet zone of Pass , and so on. (Available only when multiple passes are specified in the Fluid

Zones tab.)

Plot NTU

plots the performance data curve for the selected heat exchanger.The performance data is supplied

through the Performance Data tab.

The Heat Transfer Data Table dialog box contains information on the number of fluid flow rates and

heat transfer data for the primary and auxiliary fluids. See Using the Ungrouped Macro Heat Exchanger

Model (p. ) for details about using this dialog box.

Controls

Number of Auxiliary Fluid Flow Rates

sets the number of auxiliary fluid flow rates.

Number of Primary Fluid Flow Rates

sets the number of primary fluid flow rates.

Auxiliary Fluid Flow Rate

sets fluid flow rates for the auxiliary fluid.

Primary Fluid Flow Rate

sets fluid flow rates for the primary fluid.

sets the heat transfer for the corresponding primary and auxiliary fluid flow rates.

Read...

allows you to read in a file containing heat transfer data.

Write...

allows you to write a file containing heat transfer data.

Read...

Write...

The NTU Table dialog box contains information on the number of fluid flow rates and NTU data for

the primary and auxiliary fluids. See Using the Ungrouped Macro Heat Exchanger Model (p. ) for

details about using this dialog box.

Controls

NTU

sets the NTU values for the corresponding primary and auxiliary fluid flow rates.

Read...

allows you to read in a file containing NTU data.

Write...

allows you to write a file containing NTU data.

The Copy From dialog box allows you to copy the setup of one heat exchanger to another.

Controls

Existing Heat Exchangers

contains a list of heat exchangers, from which you can copy the settings from one heat exchanger to

another.

The Ungrouped Macro Heat Exchanger dialog box allows you to set up the ungrouped macro heat

exchanger model. See Using the Ungrouped Macro Heat Exchanger Model (p. ) for details about

using this dialog box.

Controls

Fluid Zone

specifies the zone that represents the heat exchanger.

Model Data

contains the parameters related to the heat exchanger model.

Options

allows you to choose one of the following settings:

Model Data

Options

specifies that ANSYS Fluent should compute the auxiliary fluid inlet temperature for a specified

heat rejection.

specifies that ANSYS Fluent should compute the total heat rejection of the core for a given inlet

auxiliary temperature.

Heat Transfer Model

allows you to specify either the ntu-model or the simple-effectiveness-model for heat transfer. See

Choosing a Heat Exchanger Model (p. ) for information on the differences between these models.

contains a drop-down list of all available core porosity models.

Edit...

opens the Core Porosity Model Dialog Box (p. ).

contains the parameters for heat transfer.

Heat Transfer Data...

opens the Heat Transfer Data Table Dialog Box (p. ).This item will appear for the NTU model

only.

Auxiliary Fluid Temperature

specifies the auxiliary fluid temperature.This item will appear only for the NTU model.

Primary Fluid Temperature

specifies the gas stream temperature.This item will appear only for the NTU model.

Velocity Effectiveness Curve...

opens the Velocity Effectiveness Curve Dialog Box (p. ) in which you can define the effectiveness

of the heat exchanger core (  in Equation . in the Theory Guide).This item will appear for

simple effectiveness model only.

Geometry

contains parameters to define the macro grid.

Width

sets the width of the heat exchanger core.The Width is measured in the pass-to-pass direction.

Height

sets the height of the heat exchanger core.The Height is measured in the auxiliary fluid inlet direction.

Depth

Height

Depth

sets the depth of the heat exchanger core.

specifies the number of passes for the macro grid. (See Figure . : 1x4x3 Macros (p. ).)

Number of Rows/Pass, Number of Columns/Pass

specify the number of macro rows and columns per pass in the macro grid. (See Figure . : 1x4x3

Macros (p. ).)

View Passes

displays the macro grid. (This button becomes available after you click Apply.) The path of the auxil-

iary fluid is color-coded in the display: macro  is red and macro

is blue.

Draw Mesh

toggles between displaying and not displaying the mesh when the macro mesh is displayed (using

the View Passes button).The Mesh Display Dialog Box (p. ) opens when Draw Mesh is selected.

Update from Plane Tool

updates the Auxiliary Fluid Inlet Direction and Pass-to-Pass Direction from the plane tool orient-

ation.The Width, Height, and Depth will also be updated. See Using the Plane Tool (p. ) for inform-

ation about using the plane tool.

Auxiliary Fluid Inlet Direction (height)

specifies the direction in which the auxiliary fluid enters the heat exchanger. See Figure . : 1x4x3

Macros (p. ).

Pass-to-Pass Direction (width)

specifies the direction in which the auxiliary fluid moves at the end of each pass through the heat

exchanger. See Figure . : 1x4x3 Macros (p. ).

contains the option to specify the auxiliary fluid properties.

Auxiliary Fluid Properties Method

contains options for specifying auxiliary fluid properties.

constant-specific-heat

allows you to specific a constant value for the auxiliary fluid specific heat.

user-defined-enthalpy

allows you to specify a user-defined function for the auxiliary fluid enthalpy.

Auxiliary Fluid Specific Heat

specifies the value of

in Equation . in the Theory Guide.This value is specified only if

constant-specific-heat is selected.

Auxiliary Fluid Enthalpy UDF

allows you to specify a user-defined function for the auxiliary fluid enthalpy (see Equation . in the

Theory Guide).This option is available only when user-defined-enthalpy is selected.

sets the flow rate of the auxiliary fluid (

sets the total heat rejection (

in Equation . in the Theory Guide).This value is specified only

if Fixed Heat Rejection is selected.

Initial Temperature

sets an initial guess for the inlet temperature (

in Equation . and Equation . in the Theory

Guide).This value is specified only if Fixed Heat Rejection is selected.

sets the auxiliary fluid initial temperature (

This value is specified only if Fixed Inlet Temperature is selected in the Model Data tab.

Inlet Pressure

sets the auxiliary fluid inlet pressure.This value is specified only if user-defined-enthalpy is selected.

Inlet Quality

specifies the value of  in Equation . in the Theory Guide.This value is specified only if user-

defined-enthalpy is selected.

in Equation . in the Theory Guide.This value is specified only if user-

Apply

Apply

saves all the settings for the heat exchanger specified in the Fluid Zone list.

Delete

deletes the heat exchanger specified in the Fluid Zone list.

The Velocity Effectiveness Curve dialog box allows you to define effectiveness curve. It is opened

by clicking Velocity Effectiveness Curve... in the Ungrouped Macro Heat Exchanger Dialog Box (p. ).

Controls

Number of Points

specifies the number of data pairs in the effectiveness profile.The default value of  indicates a constant

effectiveness.

Velocity, Effectiveness

specify the data pairs for the effectiveness profile.These items are available only if the simple effective

model has been selected. Note that the Effectiveness values must be within the range of –.

The Core Porosity Model dialog box allows you to modify or define a heat exchanger core model.

This dialog box opens when you click Edit... in the Ungrouped Macro Heat Exchanger Dialog Box (p. ).

Controls

Name

specifies the name of a new heat exchanger core model.

Database

contains a drop-down list of all heat exchanger core models that are currently available.

Gas-Side Pressure Drop

contains parameters that define the air-side pressure drop.

Minimum Flow to Face Area Ratio

sets the value of  in Equation . in the Theory Guide.

Entrance Loss Coefficient

Exit Loss Coefficient

Gas Side Surface Area

Minimum Cross Section Flow Area

Core Friction Coefficient

Core Friction Exponent

Change/Create

saves the settings in the dialog box and adds the new model to the Database list.

Read...

opens The Select File Dialog Box (p. ), in which you can select an external file containing a predefined

heat exchanger core model.

The Macro Heat Exchanger Group dialog box allows you to modify or define a heat exchanger core

group.

Controls

Name

specifies the name of a new heat exchanger group.

contains a list of all the fluid zones.

HX Groups

contains list of the heat exchanger groups.

Model Data

contains all the parameters to be specified for the model.

Primary Fluid Flow Direction

gives you a choice of gas flow direction.

Width, Height, Depth

specifies the width, height and the depth of the gas flow direction.

Connectivity

allows you to define the upstream and downstream connections.

Upstream

specifies the upstream heat exchanger group.

Downstream

specifies the downstream heat exchanger group.

allows you to select either the simple-effectiveness-model or the ntu-model. See Choosing a Heat

Exchanger Model (p. ) for information on the differences between these models.

specifies whether default values are chosen for the core porosity model.

Edit...

Edit...

opens the Core Porosity Model Dialog Box (p. ) for the definition of a new core porosity model.

opens the Heat Transfer Data Table Dialog Box (p. ).This dialog box allows you to define the

heat transfer for different primary and auxiliary fluid flow rates.This item will appear for the NTU

model only.

specifies the auxiliary fluid temperature.This item will appear for the NTU model only.

specifies the gas stream fluid temperature.This item will appear for the NTU model only.

Geometry

specifies the width, height and the depth of the heat exchanger.

specifies the number of passes.

Number of Rows/Pass

specifies the number of rows per pass.

Number of Columns/Pass

specifies the number of columns per pass.

displays the macro grid. (This button becomes available after you click Set.) The path of the auxiliary

fluid is color-coded in the display: macro  is red and macro

is blue.

Draw Mesh

is blue.

Draw Mesh

Auxiliary Fluid Inlet Direction

Pass-to-Pass Direction

contains inputs to specify the properties of the auxiliary fluid.

Properties Method

specifies the method to specify the auxiliary fluid properties.You can choose from constant-specific-

heat and user-defined-enthalpy.

sets the specific heat of the auxiliary fluid (

in Equation . you choose constant-specific-heat.

Enthalpy UDF

sets the enthalpy as defined by the user-defined function selected from the drop-down list.

specifies the value of  in Equation . in the Theory Guide.

Supplementary Auxiliary Fluid Stream

specifies properties of the supplementary auxiliary stream.

Supplementary Mass Flow Rate

specifies the supplementary fluid flow rate as constant, polynomial or piecewise-linear.

Supplementary Flow Temperature

specifies the supplementary fluid temperature as constant, polynomial or piecewise-linear.

Supplementary Flow Quality

specifies the supplementary fluid quality.

Create

saves all the settings in the dialog box.

Delete

deletes the group that is selected in the HX Groups list.

Replace

changes the parameters of the already existing group that is selected in the HX Groups list.

Set...

opens the Ungrouped Macro Heat Exchanger Dialog Box (p. ), in which you can define a new heat ex-

changer core model or read one from an external file.

The Species Model dialog box allows you to set parameters related to the calculation of species

transport and combustion. For details about the items below, see the following sections:

Enabling Species Transport and Reactions and Choosing the Mixture Material (p. )

Manual Inputs for Wall Surface Reactions (p. )

User Inputs for Particle Surface Reactions (p. )

Using the Premixed Combustion Model (p. )

Using the Partially Premixed Combustion Model (p. )

Steps for Using the Composition PDF Transport Model (p. )

Controls

Model

Controls

Model

indicates which model, if any, is used to calculate species transport/combustion.

Off

disables species calculations.

Species Transport

enables the calculation of multi-species transport (either non-reacting or reacting, depending on the

selection for Reactions). See Modeling Species Transport and Finite-Rate Chemistry (p. ) for details.

Non-Premixed Combustion

enables the calculation of turbulent reacting flow using the non-premixed combustion model. See

Modeling Non-Premixed Combustion (p. ) for details.This option is available only for turbulent

flows using the pressure-based solver.

Premixed Combustion

enables the premixed turbulent combustion model. See Modeling Premixed Combustion (p. ) for

details.This option is available only for turbulent flows using the pressure-based solver.

Partially Premixed Combustion

enables the partially premixed turbulent combustion model. See Modeling Partially Premixed Com-

bustion (p. ) for details.This option is available only for turbulent flows using the pressure-based

solver.

Composition PDF Transport

enables the composition PDF transport model. See Modeling a Composition PDF Transport Prob-

lem (p. ) for details.This option is available only for turbulent flows using the pressure-based

solver.

Reactions

contains options related to the modeling of reacting flow. (This section of the dialog box appears only

when Species Transport or Composition PDF Transport is the specified Model.)

Volumetric

enables the calculation of reacting flow using the finite-rate formulation. See Volumetric Reac-

Wall Surface

enables the calculation of wall surface reactions. See Wall Surface Reactions and Chemical Vapor De-

position (p. ) for details.This item will appear only if Volumetric is enabled.

Particle Surface

enables the calculation of particle surface reactions. See Particle Surface Reactions (p. ) for details.

This item will appear only if Volumetric is enabled.

Electrochemical

enables the calculation of electrochemical reactions. See Electrochemical Reactions (p. ) for details.

Integration Parameters...

is a command button that opens the Integration Parameters Dialog Box (p. ).This button appears

for the species transport model, when Volumetric is enabled under Reactions and Stiff Chemistry

Solver is enabled under Options or when Eddy-Dissipation Concept is enabled under Turbulence-

Chemistry Interaction.

Wall Surface Reaction Options

contains additional options for wall surface reactions.This portion of the dialog box appears only if Wall

Surface is enabled under Reactions.

Heat of Surface Reactions

(if enabled) includes the heat release due to surface reactions in the energy equation.You must re-

member to set appropriate formation enthalpies (standard state enthalpies) if you enable this option.

Mass Deposition Source

(if enabled) includes the effect of surface mass transfer in the continuity equation.

Aggressiveness Factor

is a numerical factor that controls the robustness and the convergence speed.This value ranges

between  and , where  is the most robust, but results in the slowest convergence.The default

Chemistry Solver

is a drop-down list in which you can select the solver for the chemically reactive flow simulation.This

item appears only for Species Transport and Composition PDF Transport models involving Volumetric

enables efficient integration of stiff chemical kinetics.This item appears only when Finite-Rate/No

TCI or Eddy-Dissipation Concept is selected in the Turbulence-Chemistry Interaction group box.

See Solution of Stiff Chemistry Systems (p. ) for details.

enables the integration of chemical kinetics using the ANSYS CHEMKIN-CFD Solver, designed for large,

stiff chemistry mechanisms.This item appears only when Finite-Rate/No TCI or Eddy-Dissipation

Concept is selected in the Turbulence-Chemistry Interaction group box.

Relax to Chemical Equilibrium

enables efficient modeling of chemical kinetics effects based only on equilibrium calculation and as-

sumptions about characteristic timescales for approaching equilibrium.This item is not available for

the Eddy Dissipation Concept TCI option. (See The Relaxation to Chemical Equilibrium Model for

details.

None - Explicit Source

makes explicit use of chemistry source terms in the species transport equations, without a stiff-

chemistry solver (not recommended for stiff or complex chemistry).

Options

contains additional options for the Species Transport model and for the Composition PDF Transport.

(This section will not appear in the dialog box for the other models.)

Inlet Diffusion

Options

includes the diffusion flux of species at inlet.

Diffusion Energy Source

(if enabled) includes the effect of enthalpy transport due to species diffusion in the energy equation.

Full Multicomponent Diffusion

enables the full multicomponent diffusion model. See Full Multicomponent Diffusion (p. ) for details.

enables the thermal diffusion model. See Thermal Diffusion Coefficients (p. ) for details.

Liquid Micro-Mixing

is used to model liquid reactions.When the Liquid Micro-Mixing model is invoked, ANSYS Fluent

uses the volume-weighted-mixing-law formula to calculate the density.

Species Migration

(if enabled) includes the ion species migration term in the species transport equation.This item appears

only when Electrochemical reactions are enabled.

Thickened Flame Model

enables the modeling of laminar flames.This application is typically used as an LES combustion

model for turbulent premixed and partially-premixed flames.

Include Temperature Fluctuations

enables the calculation of the multi-mode energy equation.This option is available when the com-

position PDF transport model is selected.

Mixture Properties

contains controls and information about the mixture being modeled.This section of the dialog box will

not appear if Premixed Combustion is the selected under Model.

Mixture Material

contains a drop-down list of available mixture materials.When you first enable the Species Transport

model, you can choose from all of the mixture materials defined in the database, or you can choose

a “template” and define your own material. (Click View... to open the Fluent Database Materials Dialog

Box (p. ) and check the properties of the mixture material selected in the list.) See Enabling Species

Transport and Reactions and Choosing the Mixture Material (p. ) for details.

When you use the Non-Premixed Combustion or Partially Premixed Combustion model,

this list will be inactive. The mixture material for a non-premixed or partially premixed combus-

tion calculation will be determined from the content of the PDF file generated in ANSYS Fluent

using the PDF Options parameters.

Number of Volumetric Species

specifies the number of gas-phase species in the selected Mixture Material.This is an informational

display only; you cannot edit this value.

Number of Solid Species

specifies the number of solid species defined in the selected Mixture Material.This is an informational

display only; you cannot edit this value. (This list will appear only for Species Transport models in-

volving Wall Surface reactions.)

Number of Site Species

specifies the number of site species defined in the selected Mixture Material.This is an informational

indicates which model is to be used for turbulence-chemistry interaction when the Species Transport

model with Volumetric reactions is used.

the two.

Guide).

Eddy-Dissipation Concept

(for turbulent flows) models turbulence-chemistry interaction with detailed chemical mechanisms

(see Equation . and Equation . in the Theory Guide).

Coal Calculator...

opens the Coal Calculator Dialog Box (p. ).

Select Boundary Species...

opens the Select Boundary Species dialog box (see Figure . :The Select Boundary Species Dialog

Box (p. )).

Select Reported Residuals

opens the Select Residual Monitored Species dialog box (see Figure . :The Select Residual

Monitored Species (p. )).

Options

contains parameters related to the laminar finite-rate or the eddy-dissipation concept model.This section

of the dialog box will appear when Finite-Rate/No TCI or the Eddy-Dissipation Concept is selected for

Turbulence-Chemistry Interaction.

Flow Iterations Per Chemistry Update

(steady-state only) specifies how often ANSYS Fluent will update the chemistry during the calculation.

Increasing the number can reduce the computational expense of the chemistry calculations.This

option is not available when the None - Explicit Source  option is selected for Chemistry Solver.

(steady-state only) is a numerical factor that controls the robustness and the convergence speed.This

value ranges between  and , where  is the most robust, but results in the slowest convergence.

The default value for the Aggressiveness Factor is ..This option is available only when Stiff

Temperature Threshold

(steady-state only) is the threshold for cell temperature below which the chemistry reaction rate in

the cell will be set to zero.This may improve the computational time without sacrificing accuracy.

The default value is  K.This option is available only when Stiff Chemistry Solver or CHEMKIN

CFD Solver is selected for Chemistry Solver.

Volume Fraction Constant

Time Scale Constant

Thickened Flame Model Options

contains parameters related to the thickened flame model.This group box is displayed only if the

Thickened Flame Model is enabled in the Options group box.

Number of Grid Points in Flame

by default are  grid points.

Integral Length Scale

is the representative of the largest eddy sizes,

in Equation . in the Fluent Theory Guide (typically,

/ to / of a characteristics dimension, such as a burner diameter, an inlet diameter, or a size of a

bluff body).This item is available only for simulations with the Large Eddy Simulation (LES) turbulence

model.

PDF Options

contains options related for the non-premixed combustion model. (This section will appear only if Non-

Premixed Combustion or Partially-Premixed Combustion is the selected Model.)

can be enabled to account for cases where substantial pressure changes occur in time and/or space

when modeling a non-adiabatic system. See Specifying the Operating Pressure for the System (p. )

Probability Density Function

is a drop-down list that allows you to choose between the shape of the assumed probability density

function (PDF):

This control appears after you generate or read a PDF table into ANSYS Fluent.

Chemistry

tab contains the parameters to define problems using the chemistry model. See Setting Up the Equilibrium

Chemistry Model (p. ) for details.

State Relation

Chemical Equilibrium

enables the equilibrium chemistry model. See Setting Up the Equilibrium Chemistry Model (p. )

Steady Diffusion Flamelet

enables the steady diffusion flamelet model. See The Diffusion Flamelet Models Theory in the

Unsteady Diffusion Flamelet

enables the Eulerian unsteady diffusion flamelet model.

Diesel Unsteady Flamelet

enables the diesel unsteady laminar flamelet model. See Using the Diesel Unsteady Laminar

Flamelet Model (p. ) for details.

Flamelet Generated Manifold

enables the flamelet generated manifold (FGM) model.This is available when the Partially Pre-

mixed Combustion model is selected. See Partially Premixed Combustion in the Theory Guide for

details.

Energy Treatment

Adiabatic

enables adiabatic modeling options for the problem.

Non-Adiabatic

enables non-adiabatic modeling options for the problem. See Non-Adiabatic Extensions of the

Non-Premixed Model in the Theory Guide for details.

Coal Calculator

Stream Options

contains the parameters for the equilibrium chemistry model or the steady diffusion flamelet model.

Secondary Stream

includes the secondary inlet stream in the model.

Empirical Fuel Stream

enables parameters to define fuel stream empirically.This option is available only with the full

equilibrium chemistry model.

Empirical Secondary Stream

enables parameters to define secondary stream empirically.This option is available only with the

full equilibrium chemistry model.

Model Settings

contains a list of parameter settings.

specifies the system operating pressure used to calculate the density using the ideal gas law. See

Specifying the Operating Pressure for the System (p. ) for details.

Fuel Stream Rich Flammability Limit

specifies the rich flammability limit for fuel stream when the equilibrium chemistry option is used.

You will not set these if you have used the empirical definition option for fuel composition. See

Enabling the Rich Flammability Limit (RFL) Option (p. ) for details.

Secondary Stream Flammability Limit

specifies the rich flammability limit for secondary stream when the equilibrium chemistry option

is used.You will not set these if you have used the empirical definition option for fuel composition.

See Enabling the Rich Flammability Limit (RFL) Option (p. ) for details.

Empirical Fuel Lower Calorific Value

specifies the lower calorific value of fuel stream.

Empirical Fuel Specific Heat

specifies the specific heat value of fuel stream.

Empirical Fuel Molecular Weight

specifies the molecular weight of the fuel stream.

Empirical Secondary Lower Calorific Value

specifies the lower calorific value of secondary stream.

Empirical Secondary Specific Heat

specifies the specific heat value of secondary stream.

Empirical Secondary Molecular Weight

specifies the molecular weight of the secondary stream.

Options

contains options related to the steady flamelet model.

Create Flamelet

enables the Import CHEMKIN Mechanism... button that opens the Import CHEMKIN Format

Mechanism Dialog Box (p. ) where you can import the CHEMKIN mechanism and thermody-

namic data, to create a flamelet file.This option is available for the steady flamelet model. See

Setting Up the Steady and Unsteady Diffusion Flamelet Models (p. ) for details.

Import Flamelet

enables the Import Flamelet File... button that opens The Select File Dialog Box (p. ) where

you can select the existing flamelet in ANSYS Fluent.You can also set the file type parameters to

import the existing flamelet in ANSYS Fluent. See Setting Up the Steady and Unsteady Diffusion

Flamelet Models (p. ) for details.This option is available for the steady flamelet model.

Flamelet Type

gives you the option of creating a Premixed Flamelet or a Diffusion Flamelet.This is available when

the Flamelet Generated Manifold model is selected.

Flamelet Solution Method

allows you to solve the premixed FGM either in the CHEMKIN Physical Space or in the Progress

Variable Space.This is available when the Flamelet Generated Manifold state reaction is selected

and Premixed Flamelet is selected as the Flamelet Type.

File Type

contains the toggle buttons for two flamelet file types.

Standard

enables the import of an ASCII format standard flamelet file.

CFX-RIF

enables the import of an ASCII format CFX-RIF flamelet file.

Flamelet Property File Name

opens The Select File Dialog Box (p. ) in which you can save the existing flamelet in ANSYS Fluent to

use when running an existing case.

Thermodynamic Database File Name

specifies a path for the thermodynamic database file to be read.

Boundary

tab contains the list of boundary species and related parameters.This is available only for equilibrium

chemistry model. See Defining the Stream Compositions (p. ) for details.

Species

contains the list of the species used in the problem.

Fuel

specifies the fuel species.

Oxid

specifies the oxidizing species.

Second

specifies the secondary species.

Boundary Species

allows you to specify the species you want to add or remove from the model.You can type the species

chemical formula in the field below it.

Add

adds the species in the model.

Remove

removes the species from the model.

List Available Species

prints a list of all species in the thermodynamic database file (thermo.db) in the console window.

Remove

specifies the temperature of different streams that you have defined.

Fuel

is the temperature of the fuel inlet in the model.

Oxid

is the temperature of the oxidizer inlet in the model.

Second

is the temperature of the secondary stream inlet in the model.

Specify Species in

allows you to define the unit of species concentration.

allows you to specify the species in terms of mass fraction.

allows you to specify the species in terms of mole fraction.

Control

tab contains the parameters for exclusion and inclusion of equilibrium species.This is available only for

equilibrium chemistry model. See Forcing the Exclusion and Inclusion of Equilibrium Species (p. ) for

details.

Species Excluded from Equilibrium

lists the species excluded from equilibrium calculation.

Species

lists the slow-forming species that are zeroed in the initial flamelet profile.

Add

allows you to add equilibrium species.

Remove

allows you to remove equilibrium species.

prints a list of all species in the thermodynamic database file in the console window.

Flamelet Controls

allows you to adjust the controls for the flamelet solution. Note that the Create Flamelet option in

the Chemistry tab must be selected for the Steady Diffusion Flamelet or Flamelet Generated

Manifold models for these controls to be available.

Initial Fourier Number

sets the first time step for the solution.

Fourier Number Multiplier

increases the time step at subsequent times. Every time step after the first is multiplied by this

value.

value.

Relative Error Tolerance and Absolute Error Tolerance

specifies the local error controls during numerical integration.

Flamelet Convergence Tolerance

specifies the maximum absolute change in species fraction or temperature at any discrete mixture-

fraction.

Maximum Integration Time

specifies the maximum total elapsed time for flamelet calculation. ANSYS Fluent will stop the

flamelet calculation after the total elapsed time has exceeded this value.

Flamelet

tab allows you to adjust the controls for the flamelet solution. See Defining the Flamelet Controls (p. )

Flamelet Parameters

consist of the controls for the flamelet solution.

Note

The parameters may vary slightly if you selected the Flamelet Generated Manifold

model (see Flamelet Generated Manifold (p. ) for those specific parameters).

) and

the fuel (

).

specifies the maximum number of laminar flamelet profiles to be calculated.

is the scalar dissipation of the first flamelet in the library.

specifies the ratio of the scalar dissipation step in which successive flamelets are generated when

the scalar dissipation is less than  s-.This corresponds to

for <  in Equation . in the

Theory Guide.This option is available with the Steady Diffusion Flamelet model and Diffusion

FGM only.

FGM only.

specifies the interval between scalar dissipation values (in s-) for which multiple flamelets will

be calculated.This corresponds to

for ≥  in Equation . in the Theory Guide.This option

is available with the Steady Diffusion Flamelet model and Diffusion FGM only.

enables you to hook a user-defined function for scalar dissipation and mean mixture fraction (or

progress variable) grid discretization

Unsteady Flamelet Parameters

consist of the controls for the unsteady flamelet solution.

) and

the fuel (

).

is the limit at which the unsteady flamelet model temporally convects and diffuses a marker

probability equation through a steady-state ANSYS Fluent flow-field.

is where flamelets extinguish at large scalar dissipation (mixing) rates.

is the number at which ANSYS Fluent automatically selects the time step for the probability

equation based on this convective Courant number.

specifies the number of unsteady laminar flamelets that ANSYS Fluent will automatically generate

during the simulation.

determines whether the equilibrium assumption is used to compute the progress variable (Equa-

tion . in the Fluent Theory Guide). If this option is selected, ANSYS Fluent will compute the progress

variable using equilibrium. Otherwise, the progress variable will be computed using the solution of

flamelet generated with initial scalar dissipation as a denominator in Equation . in the Fluent Theory

Guide This option is available only with the diffusion FGM model.

change of slopes, between successive grid points is less than user-specified tolerances. Once this

option enabled, you can specify the following parameters:

Initial Number of Grid Points in Flamelet: calculates a steady solution on a coarse grid.

Maximum Change in Value Ratio: is

Maximum Change in Slope Ratio: is

Refine flamelet based on: allows you to select either the Stoichiometric mixture fraction or

Specified mixture fraction. For Specified mixture fraction, you must also specify a mixture fraction

level at which the flamelet is solved during the grid refinement.This option is available for the

premixed FGM model only.

Set Flamelet Parameters

opens Unsteady Flamelet Parameters Dialog Box (p. ).

Calculate Flamelets

begins the laminar flamelet calculation.

Display Flamelets...

opens the Flamelet 3D Surfaces Dialog Box (p. ) from which you can display 2D plots and 3D surfaces

showing the variation of species fraction or temperature with the mean mixture fraction or scalar

dissipation.

Initialize Unsteady Flamelet Probability

initializes the unsteady flamelet and its probability marker equation.

Display Unsteady Flamelet...

opens the Flamelet 2D Curves Dialog Box (p. ) from which you can display 2D plots of the different

variables.

Table

tab contains parameters to create the look-up table. See Calculating the Look-Up Tables (p. ) for details

of the items listed below.

Note

If you selected the Flamelet Generated Manifold model, the parameters will be different.

See Calculating the Look-Up Tables (p. ) for those specific parameters.

Table Parameters

consists of the controls for the lookup table. A different set of parameters for you to enter will be

displayed if Automated Grid Refinement is enabled or disabled.

variance, and mean enthalpy (for non-adiabatic systems).

specifies the maximum number of grid points used for tabulation.The grid refinement procedure

will stop inserting the points when either the change in value and slope between successive

points is within tolerance or the maximum number of grid points are generated.

specifies the maximum allowable change in value of table variables between successive grid

points as specified by Equation . in the Theory Guide.

specifies the maximum change in the slope of table variables between successive grid points as

specifies the minimum temperature in the lookup tables.

is the number of discrete values of  at which the look-up tables will be computed.

at which the look-up tables will be computed.This option

is available only when a secondary stream has been defined.

is available only when no secondary stream has been defined.

is the maximum number of species that will be included in the look-up tables.

is the number of discrete values of enthalpy at which the three-dimensional look-up tables will

be computed.This input is required only if you are modeling a non-adiabatic system.

is used to determine the lowest temperature for which the look-up tables are generated (see

Figure . :Visual Representation of a Look-Up Table for the Scalar as a Function of Mean Mixture

Fraction and Mixture Fraction Variance and Normalized Heat Loss/Gain in Non-Adiabatic Single-

Mixture-Fraction Systems in the Theory Guide).This option is available only if you are modeling

a non-adiabatic system.

is an adaptive algorithm that inserts grid points in all table dimensions so that changes in the values

of tabulated variables (such as mean temperature, density and species mass fractions) between suc-

cessive grid points, as well as changes in their slopes, are less than a user specified tolerance.

) will be generated in ANSYS Fluent and appended

to the flamelet library before the PDF table is calculated.This option is available only with the steady

diffusion flamelet model.

FGM Scalar Transport

opens the Select Transported Scalars Dialog Box (p. ).

Calculate PDF Table

generates the look-up table.

Display PDF Table

opens the PDF Table Dialog Box (p. ) where you can display 2D plots and 3D surfaces showing the

variation of species mole fraction, density, or temperature with the mean mixture fraction, mixture

fraction variance, or enthalpy.

tab contains parameters needed to modify the piecewise-linear points. See Modifying the Unburnt Mixture

Property Polynomials (p. ) for the details.

Partially Premixed Mixture Properties

contains the list of properties that you can modify. Edit... opens the Quadratic Mixture Fraction

dialog box where you can modify the values of the polynomial coefficients.

For each polynomial function of  under Partially Premixed Mixture Properties you can click

Edit... and specify values for Coefficient , Coefficient , Coefficient , and Coefficient  in

the appropriate Quadratic of Mixture Fraction dialog box.

Non-Adiabatic Laminar Flame Speed

when enabled includes the non-adiabatic effects on the laminar flame speed by tabulating the lam-

inar speeds in the PDF table. See Laminar Flame Speed in the Theory Guide.

Recalculate Properties

will calculate the partially premixed properties.

Premix

tab contains options and parameters for the Turbulent Flame Speed Model, the Variance Settings,

and the Turbulence-Chemistry Interaction.

Note

Premix

Note

Note that the Turbulent Flame Speed Model controls are available for both premixed

and partially premixed combustion models. However, for the partially premixed combus-

tion model, they are organized in the Premix tab.

Turbulent Flame Speed Model

allows you to select the Flame Speed Model and specify its parameters.This section will appear only

if Premixed Combustion or Partially Premixed Combustion is the selected Model and if the C

Equation or G Equation premixed model is chosen.

Flame Speed Model

is a drop-down list in which you can select the turbulent flame speed model.You can choose

between zimont (see Zimont Turbulent Flame Speed Closure Model in the Fluent Theory Guide)

and peters (see Peters Flame Speed Model in the Fluent Theory Guide).

Turbulent Length Scale Constant

(zimont model) specifies the value of

Turbulent Flame Speed Constant

(zimont model) specifies the value of  in Equation . in the Theory Guide.

Stretch Factor Coefficient

Wall Damping Coefficient

in Equation . (premixed combustion model) or in Equation . in

the Fluent Theory Guide (partially premixed combustion model).

(zimont model) is the modeling constant in the RANS region (

Guide).This option is available for the Partially Premixed Combustion model with the SBES model

only.

only.

(zimont model) is the modeling constant in the RANS region (  in Equation . in the Theory

only.

Ewald Corrector

(peters model) is enabled by default and described in Peters Flame Speed Model.

Blint Modifier

(peters model) enables/disables Blint's correlation for laminar flame thickness  (used in Equa-

tion . thru Equation . in the Fluent Theory Guide). See Peters Flame Speed Model in the

G Equation Settings

allows you to select either the transport equation or algebraic option for the calculation of the

flame distance variance. Consult Peters Flame Speed Model in the Theory guide for the variance

transport and algebraic equation expressions (Equation . and Equation . ).

Flame Curvature Source

includes the curvature source term in the G-Equation, which is the last term in Equation ..

(partially-premixed combustion FGM model only) allows you to choose between Finite-Rate and

Turbulent Flame Speed. For more information about these models, see FGM Turbulent Closure in

is available for the G Equation premixed or partially premixed model and C Equation partially premixed

FGM model.

Variance Method

is a drop-down list that allows you to choose between transport equation and algebraic. If the

SBES model is enabled, you can also choose hybrid. Consult FGM Turbulent Closure in the Fluent

Theory Guide for the C Equation model (Equation . and Equation .) and G-Equation

Model Theory in the Fluent Theory Guide for the G-Equation model (Equation . and Equation . ).

for LES, and the hybrid for SBES.

Premixed Combustion Model Options

contains options for the premixed combustion model. (This section will appear only if Premixed Com-

bustion is the selected Model.)

Adiabatic

enables the adiabatic premixed combustion model, which calculates temperature using Equation .

enables the non-adiabatic premixed combustion model, which calculates temperature using Equa-

Premixed Model

contains options for choosing a premixed model.

C Equation

allows you to choose the C equation as described in C-Equation Model Theory.

Extended Coherent Flamelet Model

allows you to choose the Extended Coherent Flamelet model as described in Extended Coherent

Flamelet Model Theory.

G Equation

allows you to choose the G equation as described in G-Equation Model Theory.

Extended Coherent Flamelet Model Constants

contains model constants for the Extended Coherent Flame Model. (This section will appear only if Pre-

mixed Combustion or Partially Premixed Combustion is the selected Model and if the Extended Co-

herent Flame Model flame speed model is chosen.) See Modifying the Constants for the ECFM Flame

Speed Closure (p. ) for details. Note that for the partially premixed combustion model, Extended Co-

herent Flamelet Model Constants appear in the Premix tab.

ITNFS Treatment

contains a drop-down list of the available ITNFS treatments: constant-delta, meneveau, blint,

poinsot, and constant.

ITNFS Flame Thickness

sets the flame thickness (Equation . in the Theory Guide).

set the turbulent Schmidt number (

).

Wall Flux Coefficient

set the wall flux coefficient.

PDF Transport Options

contains options for the Composition PDF Transport combustion model. (This section will appear only if

Composition PDF Transport is the selected Model.)

Lagrangian

solves the composition PDF transport equation by stochastically tracking Lagrangian particles through

Eulerian

assumes a shape for the PDF, allowing Eulerian transport equations to be derived.

Mixing

tab contains the mixing models.

Mixing Model

contains options to specify the method for modeling molecular diffusion. (This section will appear

only if Composition PDF Transport is the selected Model.) See Particle Mixing in the Theory Guide for

details.

Modified Curl

enables the modified curl model for molecular diffusion.

IEM

enables the IEM model for molecular diffusion.

EMST

enables the EMST mixing model for molecular diffusion.

Mixing Constant

specifies the value of the mixing constant

Guide.

Boundary

tab allows you to define the fuel and oxidizer compositions.This is only available if you select Eulerian

as the PDF Transport Option.

Species

consists of the fuel species and the oxidizer.

Species

Fuel

is the mole or mass fraction of the fuel stream.The sum of mass or mole fractions of all species in the

fuel stream should be .

Oxidizer

is the mole or mass fraction of the oxidizer stream.The sum of mass or mole fractions of all species

in the fuel oxidizer stream should be .

specifies the species as a Mass Fraction or Mole Fraction.

Control

tab contains Lagrangian PDF transport parameters.

PDF Transport Parameters

allows you to set the Particles Per Cell.

sets the number of PDF particles per cell. Higher values of this parameter will reduce statistical

error, but increase computational time.

toggles the calculation of local time steps. If this option is disabled, then you will need to specify

the Time Step directly (see Equation . in the Theory Guide).This option is available for steady-

state simulations.

Mixing #

The Coal Calculator dialog box (opened by clicking Coal Calculator... in the Species Model dialog

box) automates the calculations described in Additional Coal Modeling Inputs in ANSYS Fluent (p. ).

Controls

Coal Streams

allows you to set up to three coal streams (Species Transport model only).

Number of Coal Streams

Controls

specifies the total number of coal streams.

ID

sets the ID of the coal stream for which you want to specify Coal Properties.

Coal Properties

contains inputs for the current coal stream.

is the mass fraction of Volatile, Fixed Carbon, Ash, and Moisture in the coal.

Volatile

is the fraction of the volatile component.

Fixed Carbon

is calculated as one minus the sum of the actual Volatile, Ash, and Moisture fractions.

Ash

is the fraction of ash.

Moisture

is the moisture fraction in the coal.

Ultimate Analysis (DAF)

is the mass fraction of atomic C, H, O, N and optionally S, in the Dry-Ash-Free (DAF) coal.

Mechanism

allows you to set the mechanisms.

when enabled, allows you to set the two mixture fraction model with the primary stream repres-

enting char as

, and an empirical secondary stream representing the volatiles.This is available

when using the non-premixed combustion model.

One-step Reaction

is defined in Equation . (p. ).

Two-step Reaction

involves oxidation of volatiles to CO in the first reaction and oxidation of CO to CO2 in the second

reaction, as described in Equation . (p. ).

Include SO2

when enabled, allows you to specify the atomic mass fraction of sulphur, S, which appears under

Ultimate Analysis.

Options

Wet Combustion

when enabled will enable the DPM Wet Combustion option by default in all injections created

after the OK button is clicked in the Coal Calculator dialog box.

Settings

is where you will specify the values used in the calculation.

Coal Particle Material Name

Settings

is the name of the DPM combusting particle material.The default name is coal-particle.

Coal As-Received HCV

is the higher caloric value of the coal.

Volatile Molecular Weight

is the molecular weight of pure volatiles.

CO/CO2 Split in Reaction  Products

can be used to specify the molar fraction of CO to CO2 in the first reaction of Equation . (p. ).

The default value of  implies that all carbon is reacted to CO, with no CO2 produced.

High Temperature Volatile Yield

is where the enhanced devolatization at higher temperatures can cause the volatile yield to exceed

the proximate analysis fraction.

Fraction of N in Char (DAF)

is used in calculating the split of atomic nitrogen for the Fuel NOx model.

Coal Dry Density

is used to calculate the Volume Fraction of liquid-water for the Wet Combustion option in the

Injections dialog box.

Gas Phase Reaction

lists the reaction based on your entries for the proximate and ultimate analyses.

The Integration Parameters dialog box (opened by clicking Integration Parameters... in the Species

Model dialog box) allows you to set the parameters for the integration of the chemical source term

in Equation . in the Theory Guide. See Using ISAT (p. ) for details.

Integration Method

contains options to choose the method for integration.

ISAT

enables the ISAT option and expands the dialog box to include inputs for ISAT Parameters.

Direct Integration

enables the direct integration method to integrate the chemical source term in the calculation.

ODE Parameters

contains options to specify the error tolerances.

Absolute Error Tolerance

specifies the absolute error tolerance.

Relative Error Tolerance

specifies the relative error tolerance.

ISAT Parameters

contains inputs required for ISAT integration method.

ISAT Error Tolerance

controls the numerical error in ISAT liner interpolation. Decrease this value to get accurate minor

species and pollutant predictions.

Max. Storage

is the maximum RAM used by the ISAT table, and has a default value is  MB.

Verbosity

specifies the level of detail at which you can monitor the ISAT performance.

Clear ISAT Table

purges the ISAT table.

Options

contains options to choose the method for chemistry acceleration.

Dynamic Mechanism Reduction

accelerates chemistry by reducing the chemical kinetics mechanism on-the-fly to include only important

species and reactions, with a corresponding decrease in accuracy.This method is available for Stiff

Chemistry Solver only.

when enabled, provides additional run-time improvement, with a corresponding decrease in accuracy.

This method is available for Stiff Chemistry Solver and Relax to Chemical Equilibrium only.

is a chemistry acceleration method in addition to ISAT storage-retrieval and Cell Agglomeration,

providing faster chemistry calculations with a corresponding loss of accuracy.This method is available

for Stiff Chemistry Solver only.

Dynamic Cell Clustering

enables a computationally efficient dynamic cell clustering method (DCC) that groups computational

cells of high similarity into clusters using two DCC parameters:

Max. Clusterization (default = )

Min. Clusterization (default = )

This option is enabled by default and recommended. It is available only with the CHEMKIN-

CFD Solver.

Dynamic Adaptive Chemistry

accelerates chemistry by reducing the chemical kinetics mechanism on-the-fly to locally valid smaller

mechanisms, with a corresponding decrease in accuracy.The level of accuracy is controlled by DAC

Error Tolerance.You can select the initial target species to be tracked by the DAC algorithm in the

Select DAC Target Species dialog box that opens when you click Select Target Species. See Using

Dynamic Adaptive Chemistry with ANSYS Fluent CHEMKIN-CFD Solver (p. ) for more details.

This option is available only with the CHEMKIN-CFD Solver.

Agglomeration Parameters

contains settings for the agglomeration chemistry method.

determines the size of the clusters for species. By default, the value is ..

Temperature Bin

specifies the maximum bin size for temperature.The default value is  K.

Dimension Reduction Parameters

contains settings to accelerate the chemistry.

Number of Represented Species

must be greater than  and less than the number of species in the full mechanism.The Number of

Represented Species must also be less than  minus the number of unrepresented elements (the

number of chemical elements in the unrepresented species).

Full Mechanism Material Name

is typically the name of the CHEMKIN mechanism that you imported.

Fuel/Oxidizer Species

is where the boundary and initial fuel and oxidizer, as well as product species, are set as represented

species.

Create Reduced Dimension Mixture

creates a new mixture material called reduced-dimension-mixture, which contains the repres-

ented species as well as proxy ’species’ for the unrepresented elements.

The Flamelet 3D Surfaces dialog box allows you to display 2D plots and 3D surfaces showing the

variation of species fraction or temperature with the mean mixture fraction or scalar dissipation. See

Postprocessing the Flamelet Data (p. ) for details.

indicates the type of flamelets whose surfaces will be displayed.

Plot Variable

enables you to choose temperature or species fraction as the variable to be plotted.

Plot Type

consists of options for plot type.

3D Surface

enables plotting on 3D surfaces.

2D curve on 3D surface

enables plotting of a 2D curve on a 3D surface.

Options

consists of the following parameters:

Draw Numbers Box

enables the display of a wireframe box with the numerical limits in each coordinate direction.

Write To File

enables saving the plot data to a file.

Curve Parameters

consists of controls related to plot display.

X-Axis Function

consists of the function against which the plot variable will be displayed.

enables display of plot variable against the scalar dissipation function.

Mixture Fraction

enables display of plot variable against the mixture fraction.

Constant Value of Scalar Dissipation

consists of the controls to specify the type of discretization (that is, how the flamelet data will be

sliced) for the variable that is being held constant.

Slice by

consists of the controls to specify discretization.

Index

enables you to specify discretization index of the variable that is being held constant.

Value

enables you to specify the numerical value of the variable that is being held constant.

Index

consists of the controls that are displayed when you enable Index under Slice by.

Index #

displays the index number.

Min

displays the minimum of the range of integer values that you are allowed to choose from.

Max

displays the maximum of the range of integer values that you are allowed to choose from.

Value

consists of the controls that are displayed when you enable Value under Slice by.

Value

enables you to enter the numerical value of the variable that is being held constant.

Min

Max

The Flamelet 2D Curves dialog box allows you to display or write 2D curves of the unsteady flamelet.

See Postprocessing the Flamelet Data (p. ) for details.

Options

gives you the option to plot or Write to File 2D curves.

consists of a drop-down list of variables that you can plot or write.

Plot

Options

Plot

is available by default.When the Write to File option is enabled the Plot button changes to a Write....

The Unsteady Flamelet Parameters dialog box (opened by clicking Set Flamelet Parameters in the

Flamelet tab of the Species Model dialog box) allows you to specify the initiation time of the unsteady

flamelets. See Using the Diesel Unsteady Laminar Flamelet Model (p. ) for details.

Start CA (deg)

is the time at which each unsteady laminar flamelet will be generated during your simulation.The time

is specified in terms of seconds or degrees of crank angle if the dynamic mesh is enabled.

Burnt Initial Flamelet

if enabled, sets the initial flamelet condition to a chemical equilibrium burnt state. Otherwise, the initial

flamelet condition is set to unburnt state (default).

The Flamelet Fluid Zones dialog box allows you to select the fluid zones for computing zone-averaged

pressure and scalar dissipation. The dialog box is opened by clicking Set Flamelet Fluid Zones in the

Flamelet tab of the Species Model dialog box. See Using the Diesel Unsteady Laminar Flamelet

Model (p. ) for details.

is a selectable list of the fluid zones over which the average pressure and scalar dissipation are computed.

The Select Transported Scalars dialog box (opened by clicking FGM Scalar Transport in the Table

tab of the Species Model dialog box) allows you to select the species for which transport equations

will be solved. See Calculating the Look-Up Tables (p. ) for more information about the items below.

Controls

Available Species

is a list of species available in the FGM flamelet table (either generated or imported).To add a species to

the Transported Scalars list, select it in the Available Species multiple-selection list and click Add.

Transported Scalars

is a list of selected species for which the transport equations will be solved, as described in Scalar Transport

with FGM Closure in the Fluent Theory Guide.To remove a species from the Transported Scalars list back

to the Available Species multiple-selection list, select it and click Remove.

You can display 2D plots and 3D surfaces showing the variation of species mole fraction, density, or

temperature with the mean mixture fraction, mixture fraction variance, or enthalpy. For the Flamelet

Generated Manifold (FGM) model, additional variables are available for generating plots for PDF lookup

tables. See Postprocessing the Look-Up Table Data (p. ) for details about the items below.

The PDF Table dialog box can be accessed in one of two ways:

Controls

PDF Data Type

describes the system that you are displaying.

Controls

is a drop-down list from which you can select temperature, density, or species mass fraction as the variable

to be plotted. For the FMG model, you can also select mean rate of reaction progress.

Enthalpy Slice, Adiabatic = slice number

(FGM model only) specifies the value of the enthalpy slice level. By default, the enthalpy level is fixed at

the adiabatic level displayed in the label as Adiabatic = slice number . Enthalpy slice numbers below

the adiabatic slice number are associated with heat loss, while enthalpy slice numbers above the adiabatic

slice number are associated with enthalpy gain.

(multiple flamelets only) specifies the value of the Scalar Dissipation.

Plot Type

gives you the choice of plotting a 3D surface or a slice of a 3D surface.

3D Surface

displays a 3D plot of the variation of species mole fraction, density, or temperature with the mean

mixture fraction, mixture fraction variance, or enthalpy.

2D Curve on 3D Surface

consists of a 2D curve that is a slice of a 3D surface.

Options

contains options specific to the display of 3D surfaces or 2D curves on 3D surfaces.

enabling this option displays a wireframe box with the numerical limits in each coordinate direction.

This option is available only when 3D Surface is selected.

specifies whether you want to write the plot data to a file.This option is available only when 2D Curve

on 3D Surface is selected.The Plot button changes to a Write button when this option is enabled.

Volume Parameters

(FGM model only) contains settings for selecting and fixing a discrete independent variable.

Constant Value of

contains the discrete independent variables that can be held constant in the lookup table.The choices

are Mean Reaction Progress, Scaled Reaction Progress Variance, Mean Mixture Fraction, and

Scaled Variance.

Slice by

allows you to select whether the 3D array of data points available in the look-up table will be sliced

by Index or Value.

Index/Value

contains index/values and their ranges.

allows you to specify the discretization index or numerical value of the variable that is being held

constant.

Min/Max

are the range of integer values that you are allowed to choose from or display.

Surface Parameters

contains settings where discrete independent variables are held constant and where curve parameters

are defined.

are Scaled Heat Loss/Gain, Mean Mixture Fraction, and Scaled Variance. For a two-mixture-fraction

case, the Scaled Heat Loss/Gain is the only available option. For the FGM model, this group box

contains the discrete independent variables that have not been fixed in the Volume Parameters

group box.

Slice by

constant.

Min/Max

constant.

Min/Max

Adiabatic

is the enthalpy slice index corresponding to the adiabatic case for which the enthalpy (Scaled

Heat Loss/Gain) is held constant.

allows you to specify the X-Axis Function against which the plot variable will be displayed when 2D

Curve on 3D Surface is selected.

contains the remaining discrete independent parameters that have not been fixed yet.

Constant Value of Independent Parameter

allows you to specify the type of discretization for the variable that is being held constant using

the controls in the Slice by and Index/Value group boxes.These items are similar to those de-

Display

displays the plot variable of the 3D surface.

Plot

plots the plot variable for the 2D curve on 3D surface.

Write

opens The Select File Dialog Box (p. ) where you will specify a name for the file containing plot data.

This button appears when Write To File is enabled for the 2D Curve on 3D Surface plot type.

The Spark Ignition dialog box allows you to define multiple sparks (see Spark Model (p. ) for details).

Controls

Number of Sparks

is the quantity of sparks you would like to include in your simulation.You can define up to  sparks.

On

if enabled, turns on those sparks that will be included in the simulation.

Name

is the name of the spark.You can specify a name, or use the default name.

Define...

opens the Set Spark Ignition Dialog Box (p. ).

Name

Define...

The Set Spark Ignition dialog box allows you to set the parameters related to the spark ignition

model (see Spark Model (p. ) for details).

Controls

Name

displays the name of the spark being defined.

Spark Location

contains the parameters needed to define the location and size of the spark.

X,Y, and Z-Center

specifies x, y, and z coordinates of the spark center.

Initial Radius

specifies the initial spark radius.

Spark Parameters

contains the parameters needed to define the spark.

Start Time

is the time of spark ignition initialization in seconds.When the in-cylinder model is turned on, this

control is replaced by the Start Crank Angle control.

Start Crank Angle

is the time of spark ignition initialization in crank angle degrees.When the in-cylinder model is turned

off, this control is replaced by the Start Time option.

Duration

is the duration of the spark ignition in seconds.

Energy

contains the total energy input by the spark.The default energy value is . A positive value for energy

will cause the temperature of the spark kernel to rise above the combustion process temperature.

allows you to select the turbulent flame speed model for controlling the rate at which the flame front

moves.

Turbulent Curvature

includes the effect of flame curvature as specified in Turbulent Curvature in the Fluent Theory

Guide.

Turbulent Length

neglects the effects of flame curvature on the flame speed as described in Turbulent Length in

Herweg-Maly

Guide.

calculates the turbulent flame speed using Herweg-Maly model. See Herweg-Maly in the Fluent

Laminar

specifies the turbulent flame speed as the laminar flame speed.This option can be used to apply

user-defined function (UDF) for the turbulent flame speed definition.

Flame Surface Density

allows you to specify the flame surface density as a constant value when Constant Value is selected

under ECFM Spark Model.The value of the flame surface density must be set within the spark region.

User Sigma Source

allows you to apply a custom source term to the ECFM equation within the volume of the spark ignition

kernel. For more detail about this user-defined function, refer to Hooking an ECFM Spark Source UDF

to ANSYS Fluent in the Fluent Customization Manual.This selection is available when User Defined

Sigma Source is enabled under ECFM Spark Model.

ECFM Spark Model

contains model variants used to define the value of the flame surface density.These portions of the dialog

box only appear when the Extended Coherent Flamelet Model (Setting Up the Extended Coherent

Flame Model (p. )) is selected in the Species Model dialog box.

Turbulent

takes into account flame wrinkling as described in Turbulent Model in the Fluent Theory Guide.

Zimont

operates in the same way as the spark model used with the Zimont combustion model. See Zimont

allows you to specify the Flame Surface Density.

kernel.

kernel.

The Autoignition Model dialog box allows you to set the parameters related to the Knock Model or

the Ignition Delay Model. See Modeling Engine Ignition (p. ) for details.

Controls

Model

contains options to disable or enable models.

Off

disables the model.

Knock Model

enables the knock model.With the Premixed Combustion or Partially Premixed Combustion

models selected, only the Knock Model can be turned on.

Ignition Delay Model

enables the ignition delay model.

Options

contains two correlation options that exist with each model.

Douaud

option is used for knock in spark ignition engines.The modeling parameters that are specified for

this option are the Pre Exponential, Pressure Exponent, Activation Temperature, Octane Number,

and Octane Exponent (Equation . in the Theory Guide).

Generalized

enables generalized correlation described by Equation . in the Theory Guide. It requires the same

Hardenburg

enables Hardenburg correlation, which is used for heavy-duty diesel engines.This option is enabled

only for the ignition delay model.

contains parameters related to the selected model. See Using the Autoignition Models (p. ) for the

details about the parameters in this dialog box.

Pre-Exponential

see Equation . and Equation . in the Theory Guide.

Activation Temperature

see Equation . in the Theory Guide.

Pressure Exponent

Octane Number

Octane Number Exponent

RPM Exponent

Options

contains two correlation options that exist with this model.

Douaud

enables Douaud correlation (Equation . in the Theory Guide) used for knock in SI engines.

option (Equation . in the Theory Guide) in the knock model require the same parameters as in

the ignition delay model.

The Inert dialog box allows you to set the parameters related to the inert model. For details, see Setting

Up the Inert Model (p. ).

Controls

Model

allows you to enable or disable the inert model.

Off

Inert Transport

enables the inert model.

Composition Options

allows you to select a fixed H/C ratio or to specify the composition.

Fixed H/C Ratio

allows you to specify a fixed ratio of hydrogen to carbon in the H/C Ratio field.

User Specified

allows you to specify an arbitrary composition for the inert stream.

Composition

allows you to set the H/C ratio or the mass fraction.

When Fixed H/C Ratio is selected under Composition Options, the following option(s) are available:

H/C Ratio

specifies the fixed ratio of hydrogen to carbon when the Fixed H/C Ratio option is enabled.

H/C Ratio

When User Specified is selected under Composition Options, the following option(s) are available:

Species

lists the inert species name.

displays the mass fraction of the corresponding species.

Inert Species

allows you to specify the name of the inert species.

Add

adds the specified inert species to the species list.

Remove

removes the specified inert species from the species list.

Normalize Species

makes sure the species mass fractions add up to .

lists all species in the thermodynamic database file (thermo.db) in the console window,

The NOx Model dialog box allows you to set parameters related to the NOx postprocessor. See Using

the NOx Model (p. ) for details about the items below.

Controls

Models

contains tabs for defining the models used to calculate the NOx production.

Formation

contains the parameters to define the NOx model formation.

Pathways

contains toggle buttons for enabling the NOx models to be used for the calculation of NO and

HCN concentrations.

Thermal NOx

enables calculation of thermal NOx.

Prompt NOx

enables the calculation of prompt NOx.

Fuel NOx

enables the calculation of fuel NOx.When using the non-premixed combustion model, the

Fuel NOx option is only available if the DPM model is also enabled.

N2O Intermediate

enables the formation of NOx through an N2O intermediate.This option will only appear if

one of the previously listed NOx models is enabled.

Fuel Streams

allows you to define multiple fuel streams for prompt NOx and fuel NOx formation.

Number of Fuel Streams

sets the number of fuel streams.You are allowed up to three fuel streams.

Fuel Stream ID

specifies the fuel stream you are defining in the PDF Stream drop-down list, the Fuel Species

selection list, the Prompt tab, and the Fuel tab.

PDF Stream

specifies the PDF stream species associated with a particular Fuel Stream ID, when calculating

fuel NOx formation in conjunction with the non-premixed combustion model.You can select

either the primary or secondary fuel streams, as defined in the PDF table.

Fuel Species

is a list containing all of the defined species, which allows you to specify the species that is

the fuel associated with a particular Fuel Stream ID.You cannot select more than  fuel

species for each fuel stream, and the total number of fuel species selected for all the fuel

streams combined cannot exceed . Note that when the non-premixed combustion model

is enabled, your selection in the Fuel Species list only applies to prompt NOx calculations.

Fuel Sources

is a list containing all of the fuel N sources.This list is available when Fuel NOx is enabled and

your case contains injections with different DPM materials defined, such as combusting

particles and droplets.

contains the NOx Rate drop-down list, which allows you to use a user-defined function (UDF) to

contribute to the rate of NOx production. See the separate Fluent Customization Manual for details.

Note that you may also use a UDF to specify custom values for the maximum limit (

) that is

used for the integration of the temperature PDF (when temperature is accounted for in the turbu-

) that is

lence interaction modeling).

Reduction

allows you to specify the reduction methods.

Methods

contains the list of reduction methods.

Reburn

enables the calculation of NOx reburning effects.

SNCR

enables the calculation of NOx reduction by the SNCR method.

Turbulence Interaction Mode

contains parameters related to the effect of turbulent fluctuations on the NOx formation. See NOx

Formation in Turbulent Flows in the Theory Guide for details.

PDF Mode

is a drop-down list containing options that take into account turbulent fluctuations when you

compute the specified NOx formation. See Setting Turbulence Parameters (p. ) for details.

none

specifies the use of laminar NOx rate calculations, so that the effects of turbulence are ignored.

includes fluctuations of temperature.

temperature/species

includes fluctuations of the temperature and the mass fraction of the species selected in the

Species drop-down list (which appears when you select this option).

mixture fraction

includes fluctuations of the mixture fraction(s).This is available for non-premixed combustion

calculations only.

PDF Type

allows you to specify the shape of the PDF.

beta

models the PDF using Equation . in the Theory Guide.

gaussian

PDF Points

controls the number of points at which the beta function in Equation . or Equation .

in the Theory Guide will be integrated.The default value of , which indicates that the beta

PDF Points

function will be integrated at  points on a histogram basis.The default value should yield an

accurate solution with a reasonable computation time. Increasing this value may improve accuracy,

but will also increase the computation time.This field is only available when temperature or

temperature/species is selected from the PDF Mode drop-down list.

allows you to specify the form of the transport equation that is solved to calculate the temperature

variance.

algebraic

is an approximate form of the transport equation (see Equation . in the Theory Guide).

transported

solves Equation . in the Theory Guide.

provides various options for determining the maximum limit(s) for the integration of the PDF

used to calculate the temperature.

global-tmax

sets the limit as the maximum temperature in the flow field.

local-tmax-factor

yields cell-based maximum temperature limits by multiplying the local cell mean temperature

by the value entered in Tmax Factor.

specified-tmax

sets the limit for each cell to be the value entered in Tmax.

allows you to hook a user-defined function that specifies custom values for the maximum

limit (

), which is used for the integration of the temperature PDF.This option is only

available if you have already compiled a user-defined function and selected it in the Formation

tab.

Species

is a drop-down list that appears when temperature/species is selected from the PDF Mode drop-

tab.

Species

down list. Here you will select the species whose mass fraction fluctuations will be factored into

the NOx rate calculations.

Formation Model Parameters

contains the tabs used to define the NOx pathways.

Thermal

contains parameters for modeling thermal NOx. (The contents of this tab will appear only if Thermal

NOx is enabled in the Formation tab.)

[O ] Model

is a drop-down list in which you can select the method to be used for calculation of thermal NOx.

To choose the equilibrium method, select equilibrium.To choose the partial equilibrium method,

select partial-equilibrium.To choose the predicted O concentration method, select instantan-

eous. See Method : Equilibrium Approach, Method : Partial Equilibrium Approach, and Method

: Predicted O Approach in the Theory Guide for details.

[OH ] Model

To exclude OH, select none.To choose the partial equilibrium method, select partial-equilibrium.

To choose the predicted OH concentration method, select instantaneous. See Method : Exclusion

of OH Approach, Method : Partial Equilibrium Approach, and Method : Predicted OH Approach

UDF Rate

provides options for the treatment of the NOx production specified by the user-defined function

selected in the Formation tab.

Replace Fluent Rate

replaces ANSYS Fluent’s thermal NOx rate calculations with the custom NOx rate produced

by your user-defined function.

Add to Fluent Rate

adds the custom NOx rate produced by your user-defined function to ANSYS Fluent’s thermal

Prompt

Prompt

contains parameters for modeling prompt NOx. (The contents of this tab will appear only if Prompt

NOx is enabled in the Formation tab.) The settings made in this tab will be associated with a partic-

ular fuel stream, specified in the Fuel Stream ID field in the Formation tab.

Fuel Carbon Number

specifies the number of carbon atoms per fuel molecule.

Equivalence Ratio

is the ratio of the actual fuel/air ratio to the stoichiometric fuel/air ratio.

UDF Rate

replaces ANSYS Fluent’s prompt NOx rate calculations with the custom NOx rate produced

adds the custom NOx rate produced by your user-defined function to ANSYS Fluent’s prompt

Fuel

contains parameters for modeling fuel NOx. (The contents of this tab will appear only if Fuel NOx is

enabled in the Formation tab.) The settings made in this tab will be associated with a particular fuel

stream, specified in the Fuel Stream ID field in the Formation tab.

Fuel Type

specifies the type of fuel NOx to be calculated.

Solid

enables the calculation of solid fuel NOx.

Liquid

enables the calculation of liquid fuel NOx.

Gas

enables the calculation of gas fuel NOx.

N Intermediate

allows you to specify any one of the hcn, nh3, or hcn/nh3/no as the intermediate species. See

Fuel NOx Formation in the Theory Guide for details.

Volatile N Mass Fraction

specifies the mass fraction of nitrogen in the volatiles.This parameter appears only for Solid fuel

NOx calculations.

Fuel N Mass Fraction

specifies the mass fraction of nitrogen in the fuel.This parameter appears only for Gas or Liquid

fuel NOx calculations.

Conversion Fraction

specifies the overall mass fraction of fuel N (for gas and liquid fuels), or volatile N or char N (for

solid fuels), that will be converted to intermediate species and/or product NO.

Partition Fractions

specifies the mass fraction of the converted fuel N (for gas and liquid fuels), or volatile N or char

N (for solid fuels), that will become hcn and nh3.The fraction that will become NO will be calculated

by the remainder.This option will appear only if you have selected hcn/nh3/no for the N Inter-

mediate or Char N Conversion drop-down lists.

Char N Conversion

is a drop-down list in which you can select no, hcn, nh3, or hcn/nh3/no as the species to which

the char N is converted (when you are calculating solid fuel NOx).This parameter appears only

for Solid fuel NOx calculations. See Setting Solid (Coal) Fuel NOx Parameters (p. ) for details.

Char N Mass Fraction

specifies the mass fraction of nitrogen in the char.This parameter appears only for Solid fuel

BET Surface Area

sets the BET internal pore surface area (see BET Surface Area in the Theory Guide for details) of

the particles.This parameter appears only for Solid fuel NOx calculations.

UDF Rate

UDF Rate

replaces ANSYS Fluent’s fuel NOx rate calculations with the custom NOx rate produced by

your user-defined function.

adds the custom NOx rate produced by your user-defined function to ANSYS Fluent’s fuel

N2O Path

contains the method to be used for formation of NO through an N2O intermediate. (The contents of

this tab will appear only if N20 Intermediate is enabled in the Formation tab.)

N2O Model

contains the drop-down list of available N2O models.

quasi-steady

enables the quasi-steady-state method of calculation (The transport equation for the species

N2O will not be solved).

transported-simple

enables the transported simple method of calculation (The pollutant species N2O is added in

the species list and it’s mass fraction will be calculated using the transport equations).

UDF Rate

Replace ANSYS Fluent Rate

replaces the NOx rate calculated by ANSYS Fluent using N2O intermediates with the custom

NOx rate produced by your user-defined function.

Add to ANSYS Fluent Rate

adds the custom NOx rate produced by your user-defined function to the NOx rate calculated

Reduction Method Parameters

contains tabs that allow you to define the methods of reduction. (These tabs are do not appear unless a

reduction method has been enabled in the Reduction tab.)

Reburn

allows you to define the NOx reduction when Reburn is enabled in the Reduction tab.

Reburn Model

contains the drop-down list of reburn methods.

instantaneous[CH ]

enables the instantaneous method in the Reburn Model.When you choose this method a

warning to include CH, CH2, and CH3 will be displayed.

partial-equilibrium

activates partial method in the Reburn Model.

Reburn Fuel Species

contains reburn fuel species drop-down list.

Equivalent Fuel Type

contains equivalent fuel type drop-down list.

SNCR

allows you to define the NOx reduction when SNCR is enabled in the Reduction tab.

Injection Method

contains the parameters for NOx reduction by SNCR method.

gaseous

includes ammonia or urea as a gas-phase pollutant species from the injection locations.

liquid

includes ammonia or urea as a liquid-phase pollutant species from the injection locations.

Reagent Species

allows you to specify the reagent species as either ammonia (nh3) or urea (co<nh2>)

Reagent Fraction in Stream

allows you to specify the mass fraction of the reagent in the reagent stream.The remaining mass

fraction is assumed to be water. If you enabled a secondary stream in your PDF calculation, by

default the secondary stream will act as the reagent stream. Note that the Reagent Fraction in

Stream field is only available when using the non-premixed combustion model with a liquid-

phase reagent injection.

Urea Decomposition

allows you to specify the decomposition model to use when the selected Reagent Species is

co<nh2>.

co<nh2>.

rate-limiting

specifies that the source terms be calculated according to the rates given in Table . :Two-

Step Urea Breakdown Process.

user-specified

allows you to specify the molar conversion fraction for ammonia, assuming that the rest of

the urea is converted to HNCO.

NH3 Conversion

is the mole fraction of

in the mixture of

and HNCO instantly created from the reagent

injection.The NH3 Conversion field only appears when user-specified is selected for Urea De-

composition.

The SOx Model dialog box allows you to set parameters related to the SOx postprocessor. See Using

the SOx Model (p. ) for details about the items below.

Controls

Model

contains the control to enable the model.

enables the model.

allows you to define multiple fuel streams for SOx formation.

specifies the fuel stream you are defining in the Fuel Species selection list and the Formation Model

Parameters group box.

is a list containing all of the defined species.This list is used to specify the species that is the fuel as-

sociated with a particular Fuel Stream ID, for any combustion model other than non-premixed

combustion.You cannot select more than  fuel species for each fuel stream, and the total number

of fuel species selected for all the fuel streams combined cannot exceed , the list of fuel species is

available when Gas is the selected Fuel Type.

is a list containing all of the fuel S sources.This list is available when Fuel Type is Liquid or Solid and

your case contains injections with different DPM materials defined, such as combusting particles and

droplets.

PDF Stream ID

SOx formation in conjunction with the non-premixed combustion model.

primary

indicates the primary fuel stream species, as defined in the PDF table.

secondary

indicates the secondary fuel stream species, as defined in the PDF table.

contains parameters related to the effect of turbulent fluctuations on the SOx formation. See SOx Formation

in Turbulent Flows in the Theory Guide for details.

PDF Mode

is a drop-down list containing options that take into account turbulent fluctuations when you compute

the specified

formation. See Setting Turbulence Parameters (p. ) for details.

none

specifies the use of laminar SOx rate calculations, so that the effects of turbulence are ignored.

includes fluctuations of temperature and mass fraction of the species selected in the Species

drop-down list (which appears when you select this option).

PDF Type

beta

gaussian

PDF Type

beta

gaussian

PDF Points

controls the number of points at which the beta function in Equation . or Equation . in

the Theory Guide will be integrated.The default value of , which indicates that the beta function

will be integrated at  points on a histogram basis, will yield an accurate solution with reasonable

computation time. Increasing this value may improve accuracy, but will also increase the computation

time.This field is only available when temperature or temperature/species is selected from the PDF

Mode drop-down list.

algebraic

provides various options for determining the maximum limit(s) for the integration of the PDF used

to calculate the temperature.

yields cell-based maximum temperature limits by multiplying the local cell mean temperature by

the value entered in Tmax Factor.

allows you to hook a user-defined function that specifies custom values for the maximum limit

(

), which is used for the integration of the temperature PDF.This option is only available if

you have already compiled a user-defined function and selected it in the SOx Rate drop-down

list in the User-Defined Functions group box.

Species

is a drop-down list which appears when temperature/species is selected from the PDF Mode drop-

down list. Here you will select the species whose mass fraction fluctuations will be factored into the

SOx rate calculations.

allows you to use a user-defined function (UDF) to contribute to the rate of SOx production. See the

separate Fluent Customization Manual for details. Note that you may also use a UDF to specify custom

) that is used for the integration of the temperature PDF (when tem-

perature is accounted for in the turbulence interaction modeling).

SOx Rate

allows you to select a compiled user-defined function.

UDF Rate

provides options for the treatment of the SOx production specified by the user-defined function.

replaces ANSYS Fluent’s SOx rate calculations with the custom SOx rate produced by your user-

defined function.

adds the custom SOx rate produced by your user-defined function to ANSYS Fluent’s SOx rate

Fuel Stream Settings

contains the parameters associated with a particular fuel stream of the SOx model, as specified in the

Fuel Stream ID field in the Fuel Streams group box.

Fuel Type

enables selection of the fuel.

Solid

enables the calculation of solid fuel SOx.

Liquid

enables the calculation of liquid fuel SOx.

Gas

enables the calculation of gas fuel SOx.

S Intermediate

drop-down list enables you to select intermediate species (h2s, so2, or h2s/so2).

Volatile S Mass Fraction

Gas

specifies the mass fraction of sulfur in the volatiles.This parameter appears only for Solid fuel streams.

Fuel S Mass Fraction

field sets the value for correct mass fraction of sulfur in the fuel (kg sulfur per kg fuel).This parameter

appears only for Liquid and Gas fuel streams.

specifies the overall mass fraction of the fuel S (for liquid or gas fuels), or the volatile S or char S (for

solid fuels), that will be converted to the intermediate species and/or product SO2.The S Intermediate

Conversion Fraction has a default value of .

specifies the mass fraction of the fuel S (for liquid or gas fuels), or the volatile S or char S (for solid

fuels) that will become h2s.The remainder will become SO2.This parameter only appears when you

select h2s/so2 for the S Intermediate or Char S Conversion drop-down lists.

Char S Conversion

drop-down list selects the char S conversion path as so2, h2s, or so2/h2s.This parameter appears

only for Solid fuel streams.

Char S Mass Fraction

specifies the mass fraction of sulfur in the char.This parameter appears only for Solid fuel streams.

allows you to include SOx products and intermediates.

Include SO3 Product

includes SO3 as a product in all of the fuel streams, as described in Reaction Mechanisms for Sulfur

Oxidation in the Theory Guide.

Include SH and SO Intermediaries

includes SH and SO as intermediates in all of the fuel streams, as described in Reaction Mechanisms

for Sulfur Oxidation in the Theory Guide.

[O ] Model

[O ] Model

drop-down list specifies the method by which O will be calculated in all of the fuel streams, that is,

equilibrium, partial-equilibrium, or instantaneous in the [O] Model.

[OH ] Model

drop-down list specifies the method by which OH will be calculated in all of the fuel streams, that is,

equilibrium, partial-equilibrium, or instantaneous in the [OH] Model.

Important

The Soot Model dialog box allows you to set parameters related to the soot model. See Using the

Soot Models (p. ) for details about the items below.

Controls

Model

specifies which model should be used for computing soot formation.

Off

disables the calculation of soot formation.

One-Step

enables the one-step soot model described in The One-Step Soot Formation Model in the Theory

Guide.

Two-Step

enables the two-step soot model described in The Two-Step Soot Formation Model.

Moss-Brookes

enables the Moss-Brookes soot model described in The Moss-Brookes Model in the Theory Guide.

Moss-Brookes-Hall

enables the Moss-Brookes-Hall soot model described in The Moss-Brookes-Hall Model in the Theory

Guide.This option is only available when C2H2, C6H6, C6H5, and H2 are present in the gas phase species

list.

Method of Moment

enables the Method of Moment soot model described in Setting Up the Method of Moments Soot

Species Definition

contains inputs for specifying the chemical species for your model.

Fuel

Fuel

is a drop-down list containing all of the defined species. Here you will select the species that is the

fuel for the One-Step and Two-Step models, as well as the Moss-Brookes model when a precursor

species is not identified in the defined species list.

Oxidant

oxidizer for the One-Step and Two-Step models.

Precursor from

allows you to select from a list of species, enter the correlation values of species, or enables you to

hook a user-defined function, used to define the user defined precursor species.This selection is

available when using the Moss-Brookes and Moss-Brookes-Hall models.

User Defined Precursor

allows you to hook a user-defined function to specify the user defined soot precursor.This selection

is available when using the Moss-Brookes and Moss-Brookes-Hall models.

Soot Precursor

is a selection list containing all of the possible precursor species found via a query of the defined

species list. By default, ANSYS Fluent only considers c2h2, c6h6, and c2h4 as possible precursor

species. For information about including other species in the possible precursor species search, contact

your ANSYS Fluent support engineer. From this list you will select the species that are the soot pre-

cursor species for the Moss-Brookes, Moss-Brookes-Hall, or Method of Moments models.

Surface Growth

is a selection list containing all of the possible surface growth species, as explained previously for the

Soot Precursor selection list. Here you will select the species that are the surface growth species for

the Moss-Brookes and Moss-Brookes-Hall models.

is the number of carbon atoms in the species selected in the Fuel drop-down list.This field appears

only for the Moss-Brookes and Moss-Brookes-Hall model, when user-correlation is selected in the

Precursor from drop-down list.

Fuel Hydrogen Number

is the number of hydrogen atoms in the species selected in the Fuel drop-down list.This field appears

Molecular Weight of Precursor

is the molecular weight of the precursor species.This field appears only for the Moss-Brookes and

Moss-Brookes-Hall model, when user-correlation is selected in the Precursor from drop-down list.

The default value is the weight of acetylene.

is a drop-down list you can use to define a laminar diffusion profile that relates mixture fraction to

precursor mass fraction.This field appears only for the Moss-Brookes and Moss-Brookes-Hall

model, when user-correlation is selected in the Precursor from drop-down list.

piecewise-polynomial

specifies that the precursor mass fraction is a piecewise-polynomial function of mixture fraction.

The default values used by ANSYS Fluent correspond to a methane diffusion flame simulation, in

which both the air and fuel initial temperatures are set to  K, and acetylene is assumed as the

soot precursor.These values can be revised via the Edit... button.

constant

specifies that the precursor mass fraction is a constant function of mixture fraction, the value of

constant

which is specified in the field below the Precursor Correlation drop-down list.

Edit...

opens the Piecewise-Polynomial Profile Dialog Box (p. ) when piecewise-polynomial is selected

from the Precursor Correlation drop-down list, thus allowing you to revise the default values.

Sticking Coefficients...

(only for the method of moments soot model) opens Sticking Coefficients Dialog Box (p. ) where

you can provide the correction factors to be used for calculating the nucleation rates.This button is

available only when User Precursor is the selected soot nucleation model.

contains inputs that specify how turbulent fluctuations are accounted for in the soot formation calculations

for the Moss-Brookes and Moss-Brookes-Hall models. For further details on these inputs, see Setting

Up the Moss-Brookes Model and the Hall Extension (p. ).

PDF Mode

is a drop-down list that contains the options for addressing turbulent fluctuations in the soot rate

calculations. Note that mixture fraction is the most accurate option, and should be used if it is

none

specifies the use of laminar soot rate calculations, so that the effects of turbulence are ignored.

specifies that the soot rate calculations include the effect of temperature fluctuations.

specifies that the soot rate calculations include the effect of fluctuations of temperature, as well

as fluctuations of the mass fraction of the species selected in the Species drop-down list (which

appears when you select this option).

is the most accurate option, specifying that the soot rate calculations include the effect of fluctu-

ations of mixture fraction(s). Note that this option is not available if you are using the eddy-dissip-

ation model.

PDF Type

beta

gaussian

PDF Points

controls the number of points at which the beta function will be integrated on a histogram basis. In-

creasing this number may improve accuracy, but will also increase compute time.This field is only

available when temperature or temperature/species is selected from the PDF Mode drop-down

list.

algebraic

(

(

you have already compiled a user-defined function.

Species

soot rate calculations.

Process Parameters

contains parameters that control the combustion process modeling.

Mean Diameter of Soot Particle

is the assumed average diameter of the soot particles in the combustion system. For the Two-Step

model, it is used to compute the soot particle mass

is the assumed average density of the soot particles in the combustion system. For the Two-Step

in Equation . in the Theory Guide. For

the Moss-Brookes and Moss-Brookes-Hall models, it is

in Equation . and  in Equa-

tion . in the Theory Guide.The default value supplied by ANSYS Fluent is  kg/

(as was

used in the work of Brookes and Moss  [] (p. )).

Normalization Parameter for Moments

(only for the method of moments soot model) is used to solve the normalized soot moment transport

equations to minimize the numerical errors.The default value of this input is sufficient and you may

not need to change this.

combustion rate in the One-Step and Two-Step models.The default value supplied by ANSYS Flu-

ent (.) assumes that the soot is pure carbon and that the oxidizer is O2.

ent (.) is for combustion of propane (C3H8) by oxygen (O2).

Mass of Incipient Soot Particle

is

in Equation . and Equation ., which is used in the Moss-Brookes and Moss-Brookes-

Hall model computations.The default value supplied by ANSYS Fluent ( kg/mol) is the mass of

carbon atoms. Note that for the original implementation of the Hall extension, the model assumed

this mass to be  carbon atoms.

Soot Oxidation Model

contains model options that determine the form of the soot oxidation term in the calculations of the

Moss-Brookes and Moss-Brookes-Hall models.

Fenimore-Jones

takes into account the soot oxidation due to the hydroxyl radical.

Lee

takes into account the soot oxidation due to the hydroxyl radical and molecular oxygen.

User Defined

enables you to select a user-defined function for soot oxidation rate.This selection is available when

using the Moss-Brookes and Moss-Brookes-Hall models.

Number of Moments

(only for the method of moments soot model) specifies the number of moments to be used in the

Method of Moments soot model. ANSYS Fluent will solve an equal number of moment transport equations.

The default value of three moments works reasonably well for wide range of problems.You can specify

up to six moments.

Soot Mechanism

(only for the method of moments soot model) contains soot mechanism options for soot modeling.

Detailed CHEMKIN Format

allows you to use a soot mechanism in CHEMKIN format.To use this option, you must import the soot

mechanism in a CHEMKIN format as described in Setting Up the Method of Moments Soot Model (p. ).

See Detailed Soot Mechanism in the Fluent Theory Guide and Setting Up the Method of Moments Soot

Model (p. ) for details about this option.

Built-In HACA

allows you to set up the nucleation mechanism and use the-built-in HACA surface growth and oxida-

tions mechanisms. See Built-In HACA Mechanism in the Fluent Theory Guide and Setting Up the

Method of Moments Soot Model (p. ) for details about this option.

Soot Nucleation Model

(only for the method of moments soot model) contains model options related to soot nucleation modeling.

This item is available only when Built-In HACA is selected.

Use Precursor

enables you to define the precursor species.The nucleation rates are calculated considering coagulation

between precursor species using kinetic theory.

Specify Mechanism

enables you to specify nucleation in terms of reactions.

User Defined Oxidation Rate

allows you to hook the user-defined function to specify the soot oxidation rate.This selection is available

when using the Moss-Brookes and Moss-Brookes-Hall models.

contains parameters that control the soot formation model.

in Equation . in the Theory Guide.This item appears only for the One-Step

soot model.

is the exponent  in Equation . in the Theory Guide.This item appears only for the One-Step

ratio  in Equation . in the Theory Guide. Equation . will be solved only if Equivalence

Ratio Minimum <

< Equivalence Ratio Maximum; if  is outside of this range, there is no soot

formation.This item appears only for the One-Step soot model.

is the term

and Equation .) in the Theory Guide.This item appears only for the One-Step and the Two-Step

soot models. For the Two-Step model, this input will be called Magnussen Constant for Soot and

Nuclei Combustion.

is the limiting value of the kinetic nuclei formation rate

Guide, is not included.This item appears only for the Two-Step soot model.

is the term

in Equation . in the Theory Guide.This item appears only for the Two-Step

is the term

in Equation . in the Theory Guide.This item appears only for the Two-Step soot

model.

is the term

model.

Guide.This item appears only for the Two-Step soot model.

is the term

in the kinetic nuclei formation term, Equation . in the Theory Guide.This item

appears only for the Two-Step soot model.

is , the constant in the soot formation rate equation, Equation . Two-Step soot model.

is , the constant in the soot formation rate equation, Equation . in the Theory Guide.This item

and Equation . in the Theory Guide).This item appears only for the One-Step and the Two-Step

soot models.

[OH] Model

is a drop-down list that allows you to specify the method by which the OH radical concentration is

calculated, that is, instantaneous or partial-equilibrium.This list appears only for the Moss-Brookes,

Moss-Brookes-Hall, and Method of Moments soot models.

[O] Model

is a drop-down list that specifies the method by which the O radical concentration is calculated, that

is, equilibrium, partial-equilibrium, or instantaneous.This list appears only for the Moss-Brookes

and the Moss-Brookes-Hall soot models, when you have selected partial-equilibrium for the [OH]

Model.

Important

To use the concentration of OH or O predicted by the combustion model, select

instantaneous for [OH] Model or [O] Model.

Model.

Important

Options

contains an option for modeling the effect of soot on a variable radiation absorption coefficient.This

group box will appear only when one of the radiation models in the Radiation Model Dialog Box (p. )

is active.

Soot-Radiation Interaction

enables the soot-radiation interaction model described in The Effect of Soot on the Absorption

Coefficient in the Theory Guide.

Soot Surface Growth Options

(only for the method of moments soot model) contains a parameter for modeling the soot surface growth.

is the number of sites/cm2 available on the soot surface for surface growth and oxidation reactions

with the method of moment soot model.

Enable Aggregation Model

(only for the method of moments soot model) enables the modeling of soot aggregates.This item is

available only when Built-In HACA is selected.

Critical diameter

is the value of the soot particle diameter above which the coagulation regime is switched from co-

alescent to aggregate.

Fractal dimension

is the parameter that describes the aggregate nature. For soot particles, a value between . and .

is found to be reasonably good.

The Sticking Coefficients dialog box allows you to set sticking coefficients for the soot model with

method of moments. It is opened from the Soot Model Dialog Box (p. ). See Setting Up the Method

of Moments Soot Model (p. ) for details about using this dialog box.

Controls

Species

shows the name of the species for which you specify the Value.

Controls

Species

The Mechanism dialog box allows you to set parameters related to nucleation reactions for the soot

model with method of moments. It is opened from the Soot Model Dialog Box (p. ). See Setting Up

the Method of Moments Soot Model (p. ) for details about using this dialog box.

Controls

Number of nucleation reactions

allows you to specify nucleation process as with a single or multi-step reaction mechanism. For each re-

action, you must specify all appropriate reaction parameters.

ID

displays the ID of the current nucleation reaction setup.

Reactant Species

is a drop-down list that enables you to select the species for the current nucleation reaction.

Stoich. Coefficient

specifies the stoichiometric coefficient of the reactant species in the nucleation reaction.

Rate Exponent

specifies the rate constant for the reactant species in the current nucleation reaction.

Arrhenius Rate

contains the inputs for the Arrhenius rate parameters related to the current nucleation reaction.

Pre-exponential Factor

in Equation . in the Theory Guide.The units of

(Equation . in the Theory Guide, are moles/volume-time

(for example, kmol/m3-s) and the units of the volumetric reaction rate,

Guide, are mass/volume-time (for example, kg/m3-s).

Important

It is important to note that if you have selected the British units system, the Arrhe-

nius factor should still be specified in SI units. This is because ANSYS Fluent applies

Important

no conversion factor to the value you enter for

you work in British units, as the correct conversion factor depends on your values

for

,

, and so on.

is the value for the constant

The Reactor Network dialog box allows you to set parameters related to the reactor network model

and calculate the reactor network for species transport/combustion. See Reactor Network Model (p. )

for details about using this dialog box.

Controls

Model

contains the option for enabling (or disabling) the reactor network model.

enables/disables the modeling of the reactor network.

Options

contains the options for reactor network model.This portion of the dialog box appears only if Reactor

Network Model is selected.

Import CHEMKIN Mechanism

allows you to import a detailed chemical mechanism in CHEMKIN format.

Detailed Mechanism Material Name

is a drop-down list of available mixture materials from which you can select a mixture material for

your reactor network simulation.

Number of Reactors

sets the number of reactors in which cells are grouped based on specified criteria.

Solve Temperature

specifies whether or not the reactor network algorithm solves the temperature. By default, this option

is selected.

Expert Option

when selected, displays the advanced options related to the solver settings.

Use Current Reactor Network

allows you to perform additional reactor network simulations with the existing network of connected

reactors.This option can be enabled once the Fluent solver agglomerates cells and obtains the reactor-

network solution.

Use Time Averaged Fields

enables you to select the time-averaged composition fields to be used for clustering reactors and the

time-averaged velocity fields for calculating reactor mass flux matrix.This option is available only for

unsteady simulations with enabled Data Sampling For Unsteady Statistics option.

Expert Options

contains advanced options for ODE solver and for reactor cell clustering control.This portion of the dialog

box appears only if Expert Options is selected.

ODE Relative Error Tolerance

specifies relative error control for ODE integrator.

ODE Absolute Error Tolerance

specifies absolute error control for ODE integrator.

allows you to specify tolerance to control the accuracy of the reactor network calculations.

Solver

allows you to select the solver for your simulation.The default segregated solver typically converges

faster than the coupled solver. However, if residuals stall above an acceptable tolerance, the coupled

Maximum Number of Iterations

(segregated solver only) sets the maximum number of solver iterations.

(coupled solver only) sets the maximum elapsed run time for ODE solver. ANSYS Fluent terminates

the run at this time if the residuals fail to converge.

enables the use of custom field functions (Custom Field Functions (p. )) for reactor network cell

clustering.

contains the list of available user-defined field functions from which you can select the functions for

reactor network cell clustering.This selection list will not appear if the Use Custom Field Functions

to Define Reactor Zones option is not selected.

Calculate Reactor Network

calculates a chemically reactive flow using reactor network model.

The Decoupled Detailed Chemistry dialog box allows you to postprocess slowly-forming, trace pol-

lutant species on a steady-state flow field using detailed chemical kinetic mechanisms.

Controls

Model

includes the option to enable Decoupled Detailed Chemistry.

Import CHEMKIN Mechanism...

opens the Import CHEMKIN Format Mechanism Dialog Box (p. ).

opens the Integration Parameters Dialog Box (p. ).

Original Species

are the species that are in the original case setup.

Pollutant Species

are typically slowly forming (far from chemical equilibrium), and occur at miniscule mass fractions.

The Reacting Channel Model dialog box allows you to solve reacting flow in shell and tube heat ex-

changers with long and thin channels.

Controls

Model

includes the option to Enable Reacting Channel Model.

Number of Boundary Groups

Controls

Model

allows you to group together channels with common flow direction, mixture materials, inlet compositions,

temperature, pressure, and mass flow rate in cases where you have multiple channels.

Flow Iterations per Coupling Iteration

is the number of outer flow iterations for each channel flow iteration.

Under-Relaxation Factor

is used to update the heat flux from the reacting channel. See Equation . in the Theory Guide.

Group Index

is used to identify the boundary group.

Group Settings

contains Group Settings that you will set.

Channel Walls in Group

are wall boundary zones that correspond to the reacting channels in the group.

Material

is the group material.

allows you to enable Surface Reactions and Porous Medium models and set related parameters.

Group Inlet Conditions

is where you specify the Temperature, the Flow Rate, the Pressure, and other inlet conditions of the

reacting channel group.

Flow Direction

is the X-, Y-, and Z-component of the flow at the inlets of the channels in the current group.

Species Composition

is where you will specify the inlet mass fractions of the group.

User Defined Inlet Conditions

enables you to hook a user-defined function to specify the reacting channel inlet conditions.When this

option is selected, the User Defined Function drop-down list becomes visible.

Display Reacting Channel Variables

opens the Reacting Channel 2D Curves Dialog Box (p. ) for postprocessing reacting channel variables.

The Reacting Channel 2D Curves dialog box allows you to display or write 2D curves of the reacting

channel.

Controls

Options

gives you the option to Plot, Report, or Write to File channel variables.

is used to identify the reacting channel boundary group.

Plot Reacting Channel Variables

enables the plotting of reacting channel variables.

Report Reacting Channel Outlet Average

enables the reporting of reacting channel outlet average.

Variable Name

specifies the channel variable for plotting.

contains a selectable list of channel variables for reporting.

Wall Surfaces

contains a selectable list of wall surfaces on which you can plot, report or write the selected channel

Plot

generates an X-Y plot.The Plot button is available when Plot Reacting Channel Variables is selected.

When the Write to File option is enabled, the Plot button changes to the Write... button.

Report

generates the report of the channel variables.The Report button is available when Report Reacting

Channel Outlet Average is selected.When the Write to File option is enabled, the Report button changes

to the Write... button.

The Discrete Phase Model dialog box allows you to set parameters related to the calculation of a

discrete phase of particles. See Modeling Discrete Phase (p. ) for details.

Controls

Interaction

contains parameters used for performing coupled calculations of the continuous and discrete phase flow.

Controls

See Procedures for a Coupled Two-Phase Flow (p. ) for details.

Interaction with Continuous Phase

enables a coupled calculation of the discrete phase and the continuous phase.

Update DPM Sources Every Flow Iteration

enables calculation of particle source terms at every DPM Iteration. For unsteady simulations, it is the

default and is recommended.

DPM Iteration Interval

allows you to control the frequency at which the particles are tracked and the DPM sources are updated.

Contour Plots for DPM Variables

contains options for enabling cell-averaged discrete phase variables for postprocessing.

Mean Values

enables additional cell-averaged discrete phase variables for postprocessing.

RMS Values

enables additional RMS values for several discrete phase variables for postprocessing.

Particle Treatment

contains options for choosing to treat the particles in an unsteady or a steady fashion.

Unsteady Particle Tracking

enables unsteady tracking of particles.

Track with Fluid Flow Time Step

enables the use of fluid flow time steps to inject the particles.

Inject Particles at

contains parameters to decide when to inject the particles for a new time step.

enables injection of particles for every particle time step.

Fluid Flow Time Step

enables injection of particles for every fluid flow time step.

In any case, the particles will always be tracked in such a way that they coincide with the flow

time of the continuous flow solver, as long as the Max. Number of Steps (in the Tracking

tab) used to compute a single trajectory is sufficient.

Particle Time Step Size

specifies particle time step size for the calculation.

Number of Time Steps

allows you to specify the number of time steps for the calculation.

Clear Particles

clears the particles that are currently in the domain.

Tracking

contains two parameters to control the time integration of the particle trajectory equations.

Tracking Parameters

contains parameters that control the tracking of particle trajectories. For steady-state particle tracking,

one simple rule of thumb to follow when setting the two parameters below is that if you want the

particles to advance through a domain of length , the Length Scale times the number of Max.

Number of Steps should be approximately equal to . See Integration of Particle Equation of Motion

in the Theory Guide for details about the items below.

is the maximum number of time steps used to compute a single particle trajectory via integration

of Equation . in the Theory Guide and  Equation ..The default value is , for steady-

state particle tracking and  for unsteady particle tracking.

Specify Length Scale

when enabled allows you to specify the length scale.

controls the integration time step size used to integrate the equations of motion for the particle.

It appears only when the Specify Length Scale option is enabled.

specifies the value of  in Equation . (p. ).

Physical Models

contains optional discrete phase models and their relevant parameters.

Options

contains additional models that can be included in the calculation. See Physical Models for the Discrete

Options

Phase Model (p. ) for more information.

Particle Radiation Interaction

includes the effect of radiation heat transfer to the particles (Equation . in the Theory Guide).

You will also need to define additional properties for the particle materials (emissivity and scattering

factor), as described in Description of the Properties (p. ).

This item appears only if the P- or discrete ordinates model is selected in the Radiation

Model Dialog Box (p. ).

Thermophoretic Force

enables the inclusion of a thermophoretic force on the particles as an additional force term. See

Thermophoretic Force in the Theory Guide for details.

Saffman Lift Force

enables the inclusion of Saffman’s lift force (lift due to shear) as an additional force term. See

Saffman’s Lift Force in the Theory Guide for details.

Virtual Mass Force

enables the inclusion of virtual mass forces in the particle force balance. See Including the

Virtual Mass Force and Pressure Gradient Effects on Particles (p. ) for details.

Pressure Gradient Force

enables the inclusion of pressure gradient effects in the particle force balance. See Including

the Virtual Mass Force and Pressure Gradient Effects on Particles (p. ) for details.

Erosion/Accretion

enables the monitoring of erosion/accretion rates at wall boundaries. See Monitoring

Erosion/Accretion of Particles at Walls (p. ) for details.

Pressure Dependent Boiling

allows you to switch from droplet vaporization (Law ) to boiling (Law ), as described in Enabling

Pressure Dependent Boiling (p. ).

Temperature Dependent Latent Heat

allows you to include the droplet temperature effects on the latent heat, as described in Equa-

Two-Way Turbulence Coupling

enables the effect of change in turbulent quantities due to particle damping and turbulence eddies.

DEM Collision

allows you to model DEM collision as described in Modeling Collision Using the DEM Model (p. ).

Stochastic Collision

enables the effect of droplet collisions, as described in Collision and Droplet Coalescence Model

Theory in the Theory Guide.

Coalescence

enables the effect of droplet coalescence, as described in Collision and Droplet Coalescence

Model Theory in the Theory Guide.This option is available when the Stochastic Collision option

Breakup

enables breakup for all suitable injections.You can select the breakup model and parameters, or

disable breakup, for each injection in the Set Injection Properties Dialog Box (p. ).

Child Particle Treatment

contains an option to Consider Children in the Same Tracking Step.This control appears only when

either Breakup is enabled under Options or wall-film is selected for Boundary Cond.Type in the

DPM tab of the Wall dialog box.

DEM Collision Model

contains model settings that allow you to continue your setup of the model.

Adaptive Collision Mesh Width

is enabled by default.This adjusts the width of the collision mesh to the largest parcel diameter

multiplied by the Edge Scale Factor

Edge Scale Factor

is the factor by which the width of the collision mesh is adjusted to the largest parcel diameter.

Static Collision Mesh Width

is the fixed width of the collision mesh.This appears when the Adaptive Collision Mesh Width

is disabled.

Maximum Particle Velocity

limits the maximum particle velocity to a physically plausible range.

DEM Collisions...

opens the DEM Collisions Dialog Box (p. ).This button is available at the bottom of the Discrete

Phase Model dialog box when the DEM Collision model is enabled.

UDF

contains parameters that can be used to customize the discrete phase model using a user-defined function.

See the separate Fluent Customization Manual for details about user-defined functions.

lists will show available user-defined functions that can be selected to customize the discrete phase

model.

Body Force

contains a drop-down list of user-defined functions available for including additional body forces.

contains a drop-down list of user-defined functions available for incorporating non-standard

erosion rate definitions.This item will appear only when the Erosion/Accretion option has been

enabled.

contains a drop-down list of user-defined functions available for calculating or integrating scalar

values along the particle trajectory.

Source

contains a drop-down list of user-defined functions available for modifying interphase exchange

terms.

contains a drop-down list of user-defined functions available for modifying spray collide function.

DPM Timestep

contains a drop-down list of user-defined functions available for modifying DPM time step.

Impingement Model

contains a drop-down list of user-defined functions available for modifying the impingement

model. If selected, the Impingement Model UDF will overwrite the impingement/splashing

model selected for the Lagrangian or Eulerian wall film boundary condition.This item is available

only when either wall-film is selected for Boundary Cond.Type in the DPM tab of the Wall

dialog box or the Eulerian Wall Film model is enabled.

Film Regime

contains a drop-down list of user-defined functions available for setting the film regime of particle

impingement.This item is available only when either wall-film is selected for Boundary Cond.

Type in the DPM tab of the Wall dialog box or the Eulerian Wall Film model is enabled.

Splashing Distribution

contains a drop-down list of user-defined functions available for modifying distribution of splashed

particle variables. If selected, the Splashing Distribution UDF will overwrite the impinge-

ment/splashing model selected for the Lagrangian or Eulerian wall film boundary condition.This

item is available only when either wall-film is selected for Boundary Cond.Type in the DPM tab

of the Wall dialog box or the Eulerian Wall Film model is enabled.

User Variables

lists the user input variables.

Number of Scalars

sets the number of scalar values used in the calculations with user-defined functions.

Numerics

tab gives you control over the numerical schemes for particle tracking as well as solutions of heat and

mass equations. See Numerics of the Discrete Phase Model (p. ) for details.

Tracking Options

contains parameters of solutions of heat and mass equations.

enables the solution of equations of motion within a specified tolerance.

Tolerance

is the maximum relative error that has to be achieved by the tracking procedure.

is the maximum number of step size refinements in one single integration step. If this number is

exceeded the integration will be conducted with the last refined integration step size.

Track in Absolute Frame

enables tracking the particles in the absolute reference frame.

Tracking Scheme Selection

contains parameters for selection of numerical schemes.

Automated

enables a mechanism to switch in an automated fashion between numerically stable lower order

schemes and higher order schemes, which are stable only in a limited range.

allows you to choose any of the tracking schemes.You also can combine each of the tracking

schemes with Accuracy Control. It is selectable only if Automated is switched off.

Coupled Heat-Mass Solution

enables the solution of the corresponding equations using a coupled ODE solver with error tolerance

control for the Droplet, Combusting, or Multicomponent particles. See Including Coupled Heat-

Mass Solution Effects on the Particles (p. ) for details.

Vaporizing Limiting Factors

for the Mass and Heat are set at the default values of . and ., respectively. See Including Coupled

Heat-Mass Solution Effects on the Particles (p. ) for details.

Averaging

Averaging

contains settings for node based averaging of DPM quantities. See Node Based Averaging of

Particle Data (p. ) for details.

Enable Node Based Averaging

enables node based averaging and displays additional related options. For non-DDPM cases, this

option is not available when the Linearize Source Terms is selected.

Average DPM Source Terms

enables averaging of source terms for the discrete phase.

Average in Each Integration Time Step

enables averages during each integration time step.

Average DDPM Variables

enables averaging of DDPM variables when the DDPM model is active.

Kernel Settings

contains settings for the kernel used by the node based averaging algorithm.

Averaging Kernel

selects the kernel to use for averaging

Gaussian Factor

sets the constant for the Gaussian distribution when gaussian is selected for Averaging Kernel.

Source Terms

Linearize Source Terms

enables the linearization of source terms for the discrete phase. For non-DDPM cases, this option

Parallel

contains parameters that control the compute nodes for performing discrete phase calculations in parallel.

See Parallel Processing for the Discrete Phase Model (p. ) for details.

Methods

allows you to select the mode for parallel processing.

enables cluster computing and also works on shared-memory machines.With this option, the

compute node processes themselves perform the particle work on their local partitions and

particle migration to other compute nodes is implemented using message passing primitives. No

special requirements are placed on the host machine. Note that this model is not available if the

Cloud Model option is enabled in the Turbulent Dispersion tab of the Set Injection Properties

allows you to specify parameters for performing the calculations on shared-memory multiprocessor

machines.

Hybrid

allows you to combine Message Passing (as previously described) and OpenMP for a dynamic

load balancing without migration of cells.This option enables multicore cluster computing, and

also works on shared-memory machines.When using the Hybrid option, you can control the

maximum number of threads on each machine via the Thread Control dialog box (see Controlling

the Threads (p. ) for details). Note that this option is not available if the Cloud Model option

is enabled in the Turbulent Dispersion tab of the Set Injection Properties dialog box.

Shared Memory Options

contains settings for the Shared Memory option.This group box is only available on Linux, when the

Shared Memory is selected from the Methods list.

Workpile Algorithm

specifies that the discrete phase calculations are to be performed on a shared-memory multipro-

cessor machine.

Number of Threads

specifies the number of threads to be used in performing the particle calculations. By default, this

parameter is equal to the number of compute nodes you specified for the parallel solver. (This

item appears only if Workpile Algorithm is enabled.)

Hybrid Options

contains settings for the Hybrid option.This group box is only available if Hybrid is selected from

the Methods list.

Use DPM Domain

enables the use of a separate computational domain for particle tracking, which improves load

balancing and scalability at the expense of some additional memory overhead.

The DEM Collisions dialog box allows you to manage the collision partners.

Controls

Collision Partners

contains a list from which you can select one or more collision partners in order to set, create, copy, rename,

delete, or list.

Create

creates a new collision partner and opens the Create Collision Partner Dialog Box (p. ), in which you

can enter the collision partner name.

Copy

creates a new injection with the same properties as the selected collision partner and opens the Copy

Collision Partner Dialog Box (p. ).

Rename

allows you to change the name of the collision partner. It opens the Copy Collision Partner Dialog

Box (p. ).

Delete

deletes the collision partner selected in the Collision Partners list.

List

lists the collision partners with their corresponding laws.

Set...

opens the DEM Collision Settings Dialog Box (p. ) for the collision partner selected in the Collision

Partners list.

The Create Collision Partner dialog box allows you to specify the name of the collision partner.

Controls

Name

is the name of the collision partner being created.

The Copy Collision Partner dialog box allows you to copy the selected collision partner.

Controls

Name

Controls

Name

is the name of the new collision partner copied from the selected partner.

The Rename Collision Partner dialog box allows you to rename the selected collision partner.

Controls

Name

is the new name of the collision partner selected in the list.

The DEM Collision Settings dialog box allows you to specify the collision laws of the collision partners.

Controls

Collision Pair

contains the list of created collision partners.

Contact Force Laws

is where you will define the collisions laws.

Normal

allows you to choose between spring, spring-dashpot, hertzian, and hertzian-dashpot.You can

also choose none if you do not want to include a contact force.

Tangential

allows you to choose between the friction-dhsf and friction-dshf-rolling force laws.You can also

exclude a force law, in which case you would select none.

Constants

contains the list of contact force constants. Depending on the contact force law in effect, different constants

will be visible.

The Solidification and Melting dialog box allows you to set parameters related to the solidification/melt-

ing model. See Modeling Solidification and Melting (p. ) for details about the items below.

Controls

Model

contains the option for turning on the model.

Solidification/Melting

enables/disables the modeling of solidification and/or melting.

Options

gives you the option of selecting one of two model rules.

Lever Rule

Options

Lever Rule

allows you to use the Lever rule (Equation . in the Theory Guide).

Scheil Rule

allows you to use the Scheil rule (Equation . in the Theory Guide). If you select Scheil Rule, then

you can enable Back Diffusion. Enter either a constant or a user-defined function to specify the value

of the Back Diffusion Parameter, used in Equation . to Equation . in the Theory Guide.

Refer to DEFINE_SOLIDIFICATION_PARAMS of the Fluent Customization Manual for detailed in-

formation about the user-defined function.

contains parameters related to the solidification/melting model.

Mushy Zone Constant

Include Thermal Buoyancy

includes the gravitational force due to the variation of density with temperature. Refer to Thermal

and Solutal Buoyancy in the Theory Guide for more information.

Note

This option is available only when solidification is modeled with species transport.

Include Solutal Buoyancy

includes the gravitational force due to the variation of density with the change in the species com-

position of the melt. Refer to Thermal and Solutal Buoyancy in the Theory Guide for more information.

Note

Include Pull Velocities

includes pull velocities in the model, as described in Momentum Equations and Pull Velocity for

Continuous Casting in the Theory Guide.

Compute Pull Velocities

enables the calculation of pull velocities based on the specified velocity boundary conditions, as de-

scribed in Pull Velocity for Continuous Casting in the Theory Guide.This option appears when Include

Pull Velocities is turned on.

Flow Iterations per Pull Velocity Iteration

specifies the number of times the pull velocity equations will be solved after each iteration of the

solver.This option appears when Compute Pull Velocities is turned on.

The Acoustics Models dialog box allows you to set parameters related to the acoustics model. See

Using the Ffowcs Williams and Hawkings Acoustics Model (p. ) for details about the items below.

Controls

Model

contains the option for turning on the acoustics model.

Off

disables the acoustics model.

Wave Equation

enables the wave equation model. See Using the Acoustics Wave Equation Model (p. ) for details.

Ffowcs-Williams & Hawkings

enables the Ffowcs Williams and Hawkings (FW-H) acoustics model. See Postprocessing the FW-H

Acoustics Model Data (p. ) for details.

Broadband Noise Sources

enables the broadband noise acoustics model. See Using the Broadband Noise Source Models (p. )

Export Options

contains the parameters related to exporting acoustics data.

Export Acoustic Source Data in ASD Format

enables/disables the saving of source data files in ASD format.

Export Acoustic Source Data in CGNS Format

enables/disables the saving of source data files in CGNS format.

Compute Acoustics Signals Simultaneously

enables “on-the-fly” calculation of sound.When this option is chosen, the ANSYS Fluent console

have been computed (for example, Extracting sound signals at x receiver loca-

Wave Equation Options

contains options for the wave equation.

Time-Filter Sounds Sources

enables/disables the filtering of sounds sources

Source Mask UDF

Specifies a UDF for the source mask.

Sponge Layer UDF

Specifies a UDF for the sponge layer.

Basic Shapes...

opens the Basic Shapes Dialog Box (p. ), which allows you to specify shapes for source mask and

sponge layer geometry.

Ffowcs-Williams & Hawkings Options

contains the Convective Effects option, which should be enabled for all cases dealing with external flows

around bodies.When this option is enabled, you will need to specify the proper Free Stream Velocity

and Free Stream Direction.

Define Sources...

opens the Acoustic Sources Dialog Box (p. ), which allows you to specify the acoustics sources.

Define Receivers...

opens the Acoustic Receivers Dialog Box (p. ), which allows you to specify the location of the receivers.

contains parameters related to the acoustics model.

sets the value of the far-field fluid density (

sets the speed of the sound at the far-field (

Artificial Viscosity Factor for Sponge Layer

Set the Artificial Viscosity Factor for Sponge Layer.

Free Stream Velocity

is available when the Convective Effects option for the Ffowcs-Williams & Hawkings model is en-

abled.

Free Stream Direction

abled.

is used to calculate the sound pressure level in dB.

is used to non-dimensionalize the acoustic power, giving the sound pressure level in dB (see

Fast Fourier Transform (FFT) Postprocessing (p. )). This parameter is equal to

W for

airborne sound and

W for underwater sound.

Reference Acoustic Intensity

, although this quantity is not currently used by ANSYS Fluent.

over this length in the depthwise direction using the identical source data.

is the number of times the noise source terms will be computed through the generation of

stochastic turbulent velocity field.

is the number of terms in the Fourier summation from which the turbulent velocity field and its deriv-

atives are computed.

Apply

saves the acoustics model settings.

The Acoustic Sources dialog box allows you to specify the acoustics sources. See Using the Ffowcs

Williams and Hawkings Acoustics Model (p. ) for details about the items below.

Controls

Source Zones

contains a list of zones from which you can select one or more emission (source) surfaces.

Type

contains a list of all possible types of zones from which you can select one or more types of the available

zones. If you select an available type of zone, the relevant zones will then be selected in the Source Zones

list. If you specify any valid interior zones as source surfaces, the Interior Cell Zone Selection Dialog

Box (p. ) will appear.

File Name

is used to give the names of the source data files (for example, acoustic_example_xxxx.asd,

where xxxx is the global time-step index of the transient solution) and an index file (for example,

acoustic_example.index) that will store the information associated with the source data.

Write Frequency

allows you to control how often the source data will be written.This will enable you to save disk space

if the time-step size used in the transient flow simulation is smaller than necessary to resolve the

sound frequency you are attempting to predict.

Number of Time Steps per File

allows you to write the source data to multiple files, each containing the source data for a number

of time steps specified by you.

Receivers...

The Acoustic Receivers dialog box allows you to specify the location of the acoustic receivers. See

Controls

Moving Receivers

allows you to specify the locations of the moving receivers.

Moving Receiver Settings

allows you to specify the Velocity and the Direction of the moving receivers.

Number of Receivers

allows you to specify the total number of receivers for which you want to compute sound.

Name

shows the name of the receiver. If you edit the field, the new name will take effect after you click the OK

button.

X-Coord.,Y-Coord., Z-Coord.

specifies the coordinates for each receiver. Note that because ANSYS Fluent’s acoustics model is ideally

suited for far-field noise prediction, the receiver locations you define should be at a reasonable distance

from the sources of sound (that is, the selected acoustic surface), and can fall outside of the computational

domain if needed.

Signal File Name

specifies the name of the file used to store sound pressure signals for the corresponding receivers. By

default, the files will be named receiver-.dat, receiver-.dat, and so on.

The Basic Shapes dialog box allows you to select shapes for use as source mask and sponge layer

geometry.

Controls

Region Registers

geometry.

Controls

contains a list of all registers which have been created for use as geometric shapes.

displays information about the selected region register.

Use Shape for Source Mask

enables/disables the use of the selected region register as a source mask.

Transition Thickness of Source Mask

Specifies transition thickness of source mask.

Use Shape for Sponge Layer

enables/disables the use of the selected region register as a sponge layer.

Transition Thickness of Sponge Layer

Specifies transition thickness of sponge layer.

The Interior Cell Zone Selection dialog box allows you to specify the acoustics sources. See Specifying

Source Surfaces (p. ) for details about the items below.

Controls

displays the selected interior surface.

Interior Cell Zone

contains a list of two interior cell zones, from which you will select the zone that is occupied by the

quadrupole sources.

The Structural Model dialog box allows you to enable structural model calculations as part of an in-

trinsic fluid-structure interaction (FSI) problem. For details, see Modeling Fluid-Structure Interaction

(FSI) Within Fluent (p. ).

Controls

Model

indicates which model, if any, is used for the structural model calculations.

Off

disables structural model calculations.

Linear Elasticity

enables structural calculations for the solid cell zone such that the internal load is linearly proportional

to the nodal displacement, and the structural stiffness matrix remains constant.This model is appro-

priate when the stress loading does not exceed the yield strength of the solid material.

The Eulerian Wall Film dialog box allows you to set various model and solution method controls for

the Eulerian Wall Film model. For more information, see Modeling Eulerian Wall Films (p. ).

Controls

enables/disables the use of the Eulerian Wall Film model in the calculations.

Model Options and Setup

contains controls for specific solution, discrete phase model (DPM), and material options for the Eulerian

Wall Film model.

Solution Options

includes options for enabling/disabling the momentum equation and DPM calculations.

allows the momentum equation (see Equation . in the Fluent Theory Guide) to be solved.

allows the energy equation (see Equation . in the Fluent Theory Guide) to be solved.

allows the passive scalar equation (see Equation . in the Fluent Theory Guide) to be solved.

Once you enable this option, you can set Scalar Diffusivity.

allows for the effect of discrete particle streams or discrete particles hitting a face on a wall

boundary that are then absorbed into the film. Once enabled, the Particle Splashing, Particle

Stripping, and Edge Separation options become available (see DPM Collection in the Theory

Guide (p. )). In addition, you can also set Impingement Parameters in the Wall Dialog

Box (p. ).

Box (p. ).

(available when DPM Collection is enabled) enables particle splashing globally.You can specify

splashing options on selected film wall boundaries in the Wall Dialog Box (p. ).

Particle Stripping

(available when DPM Collection is enabled) allows you to set the Critical Shear Stress, Diameter

Coefficient, and Mass Coefficient, available under Stripping Options.

Edge Separation

(available when DPM Collection is enabled) allows you to set the Critical Weber Number, Crit-

ical Angle, and Separation Model, available under Separation Options.

allows you to set the Sharp Edge Angle when handling the effects of sharp edges and the wall

film.

(available when the Eulerian Multiphase or Mixture (with Slip Velocity) model is enabled) allows

for the interaction of the wall film with a secondary phase in a multiphase flow. Once enabled,

the Phase Concentration and Phase Velocity can be set under Phase Accretion Options (see

Secondary Phase Accretion in the Theory Guide (p. )).

allows you to account for phase changes between the film material (liquid) and the gas species

(vapor).When this option is selected, you can specify the phase change parameters on the selected

film wall boundaries in the Wall Film tab of the Wall Dialog Box (p. ). (See Coupling of Wall

Film with Mixture Species Transport in the Fluent Theory Guide).

Momentum Options

are available when the Solve Momentum option is enabled.

Gravity Force

is the second term on the right hand side of Equation ., and is responsible for accelerating the

film in the direction of gravity component that is parallel to the wall.

Surface Shear Force

is the third term on the right hand side of Equation ., and is responsible for accelerating the

film in the direction of the external flow.

Pressure Gradient

is the first term on the right hand side of Equation ., and is the term accelerating the film in

the direction opposing the gradient in external pressure. For example, if a film on the surface of

a wing is being modeled and there is a high pressure region at the leading edge with low pressure

on the top of the wing, this term will tend to move a uniform film towards the low pressure region

on the top of the wing.

Spreading Term

is the

term on the right hand side of Equation ., and is responsible for spreading.This term

will accelerate the flow in the direction opposing the gradient in height, moving the film towards

regions of lower thickness.This term becomes available only when both Pressure Gradient and

Gravity Term are selected.

is the

term on the right hand side of Equation ..This term becomes available only when

Pressure Gradient is selected.

Sharp Edge Angle

allows you to account for sharp edges alongside the wall film, when the Treat Sharp Edge option is

enabled.

allows you to apply material properties to the wall film model.

Film Material

is the material assigned to the wall film.

Film Vapor Material

(available only when Phase Change is selected) is the material assigned to the wall film vapor.

is the surface tension for the designated wall film material.

Separation Options

(available when DPM Collection and Edge Separation are enabled) allows you to set DPM particle

separation options (see Film Separation in the Theory Guide (p. )).

is the critical value for the Weber number.

Separation Angle

is the critical angle, θ, that separation occurs.

Separation Model

allows you to specify one of three different models to calculate the number and diameter of the

shed particle stream at an edge once separation occurs. Available models include: Foucart (the

default, see Foucart Separation in the Theory Guide (p. )), O'Rourke (see O’Rourke Separation),

and Friedrich (see Friedrich Separation).

Random Separation

(available when DPM Collection and Edge Separation are enabled) allows the random selection

of the locations at which the newly spawn particles are injected (due to film separation) along

the edge at which the separation takes place.

Stripping Options

(available when DPM Collection and Particle Stripping are enabled) allows you to set DPM particle

stripping options (see Film Stripping in the Theory Guide (p. )).

Critical Shear Stress

is the critical value of the shear stress on the face where liquid film exists, which, when exceeded,

causes mass to be taken from the film.

Diameter Coefficient

is the value of  used in Equation . in the Theory Guide (p. ).

Mass Coefficient

Splashing Options

(available when DPM Collection and Particle Splashing are enabled) allows you to set DPM particle

splashing options (see Film Sub-Models in the Theory Guide (p. )).

Splashed Particles

is the number of splashed discrete particles.

Phase Accretion Options

(available when Phase Accretion is enabled) allows you to set secondary phase accretion options

(see Secondary Phase Accretion in the Theory Guide (p. )).

Phase Concentration

is the value of

used in Equation . in the Theory Guide (p. ).

Phase Velocity

allows you to skip the wall film solution during the gas phase solution, but keep the variables and

setup active.

allows you to initialize the wall film variables and prepare the solver for the solution procedure.The

film cannot be solved without first initializing the wall film model.

Solution Method and Control

contains controls for temporal or spatial discretization as well as wall film thickness for the Eulerian Wall

Film model.

allows you to set the temporal or spatial discretization methods.

Time

allows you to specify the temporal discretization methods. Available options include: First Order

Explicit, First Order Implicit, or Second Order Implicit.

Continuity

allows you to specify the spatial discretization methods for continuity. Available options include:

First Order Upwind, or Second Order Upwind.

Momentum

allows you to specify the spatial discretization methods for momentum. Available options include:

Momentum

Energy

Thickness Control

allows you to specify Maximum Thickness.

Time Marching and Time Step Control

allows you to set the number of sub-steps that the film model will take between time steps from the

main solver. For example, if the flow time step is . seconds and the number of time steps is set

to  in the film model, the film model will take  time steps of . so that the film time and the

flow time match at the end of the solution step. For implicit time stepping, the film model will take

additional sub iterations per implicit step, stopping the sub-step when the film residual drops below

the value set in the Sub-Iteration Stop option.

Adaptive Time Stepping

(steady-state flow) enables the adaptive time stepping method to determine the film time step

(

) using the maximum Courant number and the initial time step (see Steady Flow in the Theory

Guide (p. )).

Max. Courant Number

is the maximum value of the Courant number used to compute the film time step.

Initial Time Step

is an initial value for the time step used to compute the film time step.

Time-Step

(steady-state flow; default) is the user-specified size of the time step,

(see Steady Flow in the

Theory Guide (p. )).

Sub-Time Steps

(transient flow) is

Sub-Time Report Interval

(transient flow) specifies the number of iterations between the wall film solution reports.

Sub-Iterations

(available when either First Order Implicit or Second Order Implicit are enabled for Time under

Discretization) is the number of additional sub iterations per implicit step.

Sub-Iteration Stop

Discretization) is the point at which the sub iterations stop (when the film residual drops below

this value).

Sub-Iter Report Interval

(implicit time discretization calculation) specifies the number of sub-iterations between the wall

film solution reports.

DPM Control

(available when DPM Collection is enabled in the Model Options and Setup tab) allows you to

specify DPM-specific discretization.

Film Steps per DPM step

allows you to set how often the DPM phase is calculated for the film.

The Potential dialog box allows you to set parameters related to the electric potential field in your

model. See Using the Electric Potential Model (p. ) for details.

Controls

Potential

contains inputs related to modeling of the electric potential field.

Potential Equation

enables/disables the simulation of the electric potential field in the model.

Model Option

allows you to enable/disable the Include Joule Heating in Energy Equation option.This option

appears only if the energy equation is enabled.

The Materials task page allows you to set properties for any fluid or solid (or mixture, if applicable)

materials in your ANSYS Fluent simulation.

Controls

Materials

Controls

Materials

contains a listing of available fluid or solid (or mixture, if applicable) materials.

Create/Edit...

displays the Create/Edit Materials Dialog Box (p. ) for the selected item in the Materials list.

Delete

removes the selected material from the Materials list,

... Create/Edit Materials Dialog Box

... Fluent Database Materials Dialog Box

... Open Database Dialog Box

Materials Task Page

... User-Defined Database Materials Dialog Box

... Copy Case Material Dialog Box

... Material Properties Dialog Box

... Edit Property Methods Dialog Box

... New Material Name Dialog Box

... Polynomial Profile Dialog Box

... Piecewise-Linear Profile Dialog Box

... Piecewise-Polynomial Profile Dialog Box

... Model Options Dialog Box

... Compressible Liquid Dialog Box

... User-Defined Functions Dialog Box

... Sutherland Law Dialog Box

... Power Law Dialog Box

... Non-Newtonian Power Law Dialog Box

... Carreau Model Dialog Box

... Cross Model Dialog Box

... Herschel-Bulkley Dialog Box

... Biaxial Conductivity Dialog Box

... Cylindrical Orthotropic Conductivity Dialog Box

... Orthotropic Conductivity Dialog Box

... Anisotropic Conduction - Principal Components Dialog Box

... Anisotropic Conductivity Dialog Box

... Species Dialog Box

... Reactions Dialog Box

... Backward Reaction Parameters Dialog Box

...Third-Body Efficiency Dialog Box

... Pressure-Dependent Reaction Dialog Box

... Coverage-Dependent Reaction Dialog Box

... Reference Mass Fractions Dialog Box

... Reaction Mechanisms Dialog Box

... Site Parameters Dialog Box

... Mass Diffusion Coefficients Dialog Box

...Thermal Diffusion Coefficients Dialog Box

... UDS Diffusion Coefficients Dialog Box

...WSGGM User Specified Dialog Box

... Gray-Band Absorption Coefficient Dialog Box

... Delta-Eddington Scattering Function Dialog Box

... Gray-Band Refractive Index Dialog Box

... Single Rate Model Dialog Box

...Two Competing Rates Model Dialog Box

... CPD Model Dialog Box

... Kinetics/Diffusion-Limited Combustion Model Dialog Box

... Intrinsic Combustion Model Dialog Box

... Multiple Surface Reactions Dialog Box

... Edit Material Dialog Box

The Create/Edit Materials dialog box is used to create and modify materials. Materials can be down-

loaded from the global database or defined locally. See Physical Properties (p. ) for details about

defining material properties. Using the Create/Edit Materials Dialog Box (p. ) describes how to use

Controls

Name

shows the name of the material. If you edit this field, the new name will take effect when you click

Change/Create.

Chemical Formula

displays the chemical formula for the material.You should generally not edit this field unless you are

creating a material from scratch.

Material Type

is a drop-down list containing all of the available material types. By default, fluid and solid will be the

only choices. If you are modeling species transport/combustion, mixture will also be available. For

problems in which you have defined discrete-phase injections, inert-particle, droplet-particle, and/or

combusting-particle will also appear.

Fluent Fluid Materials

allows you to choose the fluid material for which you want to modify properties.This option is available

when fluid is selected in the Material Type drop-down list.

Fluent Solid Materials

allows you to choose the solid material for which you want to modify properties.This option is available

when solid is selected in the Material Type drop-down list.

Fluent Mixture Materials

allows you to choose the mixture material for which you want to modify properties.This option is available

when mixture is selected in the Material Type drop-down list.

Fluent Droplet Particle Materials

allows you to choose the droplet-particle for which you want to modify properties.This option is available

when droplet-particle is selected in the Material Type drop-down list.

Order Materials by

allows you to order the materials in the Materials list alphabetically by Name or alphabetically by

Chemical Formula.

Fluent Database...

opens the Fluent Database Materials Dialog Box (p. ), from where you can copy materials from the

global database into the current solver.

User-Defined Database...

opens the Open Database Dialog Box (p. ), where you can specify the user-defined database to be

used.

contains input fields for the material properties that are required for the active physical models.

Density

sets the material density.You may set a constant value, or select one of the other methods from the

drop-down list above the real number field. See Density (p. ) for instructions on setting density.

Cp (Specific Heat)

sets the constant-pressure specific heat of the material.You may set a constant value, or select one

of the other methods from the drop-down list above the real number field. See Specific Heat Capa-

city (p. ) for instructions on setting specific heat.

sets the thermal conductivity of the material.You may set a constant value, or select one of the other

methods from the drop-down list above the real number field. See Thermal Conductivity (p. ) for

instructions on setting thermal conductivity.

Viscosity

sets the viscosity of the material.You may set a constant value, or select one of the other methods

from the drop-down list above the real number field. See Viscosity (p. ) for instructions on setting

Molecular Weight

sets the molecular weight of the material. It is used to derive the gas constant of the material.

Standard State Enthalpy

specifies the formation enthalpy of a fluid material for a reacting flow. See Standard State Enthal-

pies (p. ) for details.

Standard State Entropy

specifies the standard state entropy of a fluid material for a reacting flow.This input is used only if

the fluid material is involved in a reversible reaction. See Standard State Entropies (p. ) for details.

specifies the reference temperature for the Heat of Formation.

specifies the kinetic theory parameter  for a fluid material. See Kinetic Theory Parameters (p. ) for

details.

specifies the kinetic theory parameter

for a fluid material. See Kinetic Theory Parameters (p. )

details.

specifies the absorption coefficient  for radiation heat transfer. See Radiation Properties (p. ) for

details. If you choose the wsggm-user-specified option from the drop-down list next to Absorption

Coefficient, the WSGGM User Specified Dialog Box (p. ) will open. If you choose the user-defined-

wsggm option from the drop-down list next to Absorption Coefficient, the User-Defined Functions

Dialog Box (p. ) will open.

specifies the scattering coefficient

for radiation heat transfer (only for the P-, Rosseland, DO, or

MC radiation models). See Radiation Properties (p. ) for details.

Scattering Phase Function

specifies an isotropic (by default) or linear-anisotropic scattering function. If you are using the DO

or MC models, delta-eddington and user-defined scattering functions are also available. See Radiation

Properties (p. ) for details. If you choose delta-eddington, the Delta-Eddington Scattering Function

specifies the refractive index for the material. It is used only when semi-transparent media are modeled

with the DO or MC radiation models.

Mixture Species

specifies the names of the species that make up a mixture material.To check or modify these names,

click the Edit... button to open the Species Dialog Box (p. ).This property appears only for mixture

materials.

Reaction

displays the reaction mechanism being used when you are modeling finite-rate reactions. finite-rate

appears if LaminarFinite-Rate or Eddy-Dissipation Concept is selected in the Species Model Dialog

Box (p. ), eddy-dissipation appears if Eddy-Dissipation is selected, and finite-rate/eddy-dissip-

ation appears if Finite-Rate/Eddy-Dissipation is selected.

Click Edit... to open the Reactions Dialog Box (p. ).

Mechanism

allows you to enable different reactions selectively in different geometrical zones. Click the Edit button

to open the Reaction Mechanisms Dialog Box (p. ). See Defining Zone-Based Reaction Mechan-

isms (p. ) for details.

contains a drop-down list of available methods for specifying the diffusion coefficients for the species

in a mixture material. If you select constant-dilute-appx, you will enter a constant value in the field

below. If you select dilute-approx or multicomponent, the Mass Diffusion Coefficients Dialog

Box (p. ) will open, and you can specify the coefficients there. If you select kinetic-theory, you will

need to specify the kinetic theory parameters for the individual fluid materials (species) that make

up the mixture. See Mass Diffusion Coefficients (p. ) for details about specifying mass diffusivity.

Thermal Diffusion Coefficient

contains a drop-down list of available methods for specifying the thermal diffusion coefficients for

the species in a mixture material. If you select kinetic-theory, you will need to specify the kinetic

theory materials (species) that make up the mixture. If you select specified, the Thermal Diffusion

Coefficients Dialog Box (p. ) will open, and you can specify the coefficients there. See Thermal Dif-

fusion Coefficient Inputs (p. ) for details about specifying thermal diffusion coefficients.

Density of Unburnt Reactants

sets the density (

in Equation . in the Theory Guide) of the unburnt products.

Temperature of Unburnt Reactants

sets the temperature (

Adiabatic Temperature of Burnt Products

(only for adiabatic premixed combustion models) specifies the value of the burnt products under

adiabatic conditions,

specifies the thermal diffusivity (  in Equation . in the Theory Guide) for use with the premixed

combustion model. See Modeling Premixed Combustion (p. ) for details.

specifies the thickness of the flame for which you have a choice of constant, user-defined, or diffus-

ivity-over-flame-speed.

Critical Rate of Strain

Heat of Combustion

(only for non-adiabatic premixed combustion models) specifies the value of

Thermal Expansion Coefficient

specifies the thermal expansion coefficient (  in Equation . (p. )) for use with the Boussinesq

approximation. See Steps in Solving Buoyancy-Driven Flow Problems (p. ) for details.

specifies the value of the droplet surface tension (  in Equation . in the Theory Guide).

or for the evolution of volatiles from a combusting particle. See Setting Material Properties for the

Discrete Phase (p. ) for details.

Latent Heat at NBP

is the latent heat of vaporization at the normal boiling point, available for droplet-particles. See Using

the Cubic Equation of State Models with the Lagrangian Dispersed Phase Models (p. ) for details.

Normal Boiling Point (NBP)

is given by Equation . (p. ). See Using the Cubic Equation of State Models with the Lagrangian

Dispersed Phase Models (p. ) for details.

specifies the thermophoretic coefficient (

in Equation . in the Theory Guide), and appears

when the thermophoretic force is included in the discrete phase calculation.

, at which the calculation of vaporization from a liquid droplet or devolatiliz-

ation from a combusting particle is initiated by ANSYS Fluent. See Setting Material Properties for the

, at which the calculation of the boiling rate equation is initiated by ANSYS

Fluent. See Setting Material Properties for the Discrete Phase (p. ) for details.

is the selected approach for the calculation of the vapor concentration of the components at the

surface.This can be Raoult’s law (Equation . in the Theory Guide), the Peng-Robinson real gas

model (Equation . in the Theory Guide), or a user-defined function that provides this value.

(

(

) is the fraction of a droplet particle that may vaporize via Laws  and/or  (Droplet Vaporization

(Law ) in the Theory Guide). For combusting particles, it is the fraction of volatiles that may be evolved

via Law  (Devolatilization (Law ) in the Theory Guide). See Setting Material Properties for the Discrete

is the mass diffusion coefficient,

, used in the vaporization law, Law .This input is also used to

define the mass diffusion of the oxidizing species to the surface of a combusting particle,

. See

Setting Material Properties for the Discrete Phase (p. ) for details.

, defined as a function of temperature, which is used in the vapor-

ization law, Law . See Setting Material Properties for the Discrete Phase (p. ) for details.

is the heat of the instantaneous pyrolysis reaction,

, that the evaporating/boiling species may

undergo when released to the continuous phase.The heat of pyrolysis should be entered as a positive

number for exothermic reaction and as a negative number for endothermic reaction.The default

value of zero implies that the heat of pyrolysis is not considered. See Setting Material Properties for

the Discrete Phase (p. ) for details.

Composition Averaging Coefficient

in Equation . in the Fluent Theory Guide.To assume bulk gas composition

for the physical properties in the particle vaporization and heating rates equations, select none from

the Composition Averaging Coefficient drop-down in the Create/Edit Materials dialog box, under

Properties.To enable property averaging, select constant and enter a value between  and  for

the Composition Averaging Coefficient.

= , the

composition reverts to the particle surface composition.

Important

other than , you must also specify Specific Heat, Viscosity and Thermal Conduct-

ivity for the evaporating species (in the Create/Edit Materials dialog box, under

Properties, for the corresponding fluid material of the continuous phase mixture).

material.

Temperature Averaging Coefficient

in Equation . in the Fluent Theory Guide.To assume bulk gas temperature

the Temperature Averaging Coefficient drop-down in the Create/Edit Materials dialog box, under

the Temperature Averaging Coefficient.

= , the

temperature reverts to the particle surface temperature.

Important

= , the

Important

the simulation results, you must provide accurate temperature-dependent data for the evapor-

ating vapor material.

droplets (Law ).

If you want to use the default diffusion-controlled model, retain the selection of diffusion-

controlled from the drop-down list to the right of Vaporization/Boiling Model. This will apply

To use the convection/diffusion-controlled model for vaporization select convection/diffusion-

controlled from the drop-down list. Equation . in the Theory Guide will be applied for

the calculation of the vaporization rate, and Equation . in the Theory Guide will be applied

in the particle heat transfer calculations This model is recommended when evaporation rates

are high. For slowly evaporating droplets both models are expected to give similar results.

You can select options for the vaporization/boiling model in the Model Options Dialog

Box (p. ) that opens when you click Edit... next to Vaporization/Boiling Model.

Degrees of Freedom

specifies the kinetic theory parameter , which is the number of nodes of energy storage.This para-

meter is required only if you are defining specific heat via kinetic theory. See Kinetic Theory Paramet-

ers (p. ) for details.

when the P- or DO radiation model is active and particle radiation interaction is enabled in the Discrete

Phase Model Dialog Box (p. ). See Setting Material Properties for the Discrete Phase (p. ) for details.

, due to particles in the P- or DO radiation model. Note that this property

will appear only if particle radiation interaction is enabled in the Discrete Phase Model Dialog

Box (p. ). See Setting Material Properties for the Discrete Phase (p. ) for details.

is the coefficient,

, which governs the swelling of the coal particle during the devolatilization law,

Law . A swelling coefficient of unity (the default) implies that the coal particle stays at constant dia-

meter during the devolatilization process. See Setting Material Properties for the Discrete Phase (p. )

, for the burnout reaction, in terms of mass of oxidant per mass

of char in the particle. See Setting Material Properties for the Discrete Phase (p. ) for details.

, in the coal particle (the fraction of the initial combusting particle

that will react in the surface reaction) Law . See Setting Material Properties for the Discrete

, which controls the distribution of the heat of reaction between the particle and

the continuous phase.The default value of zero implies that the entire heat of reaction is released to

the continuous phase. See Setting Material Properties for the Discrete Phase (p. ) for details.

is the heat released by the surface char combustion reaction, Law .This parameter is specified in

terms of heat release (for example, Joules) per unit mass of char consumed in the surface reaction.

See Setting Material Properties for the Discrete Phase (p. ) for details.

defines which version of the devolatilization model, Law , is being used. If you want to use the default

constant rate devolatilization model, retain the selection of constant in the drop-down list to the

right of Devolatilization Model and enter the rate constant

Select single-rate, two-competing-rates, or cpd-model in the drop-down list to choose one

of the optional devolatilization models (the single kinetic rate model, two kinetic rates model,

or CPD model, as described in Devolatilization (Law ) in the Theory Guide).

When the single kinetic rate model (single-rate) is selected, the Single Rate Model Dialog

Box (p. ) will appear; when the two competing rates model (two-competing-rates) is selected,

the Two Competing Rates Model Dialog Box (p. ) will appear; and when the CPD model

(cpd-model) is selected, the CPD Model Dialog Box (p. ) will appear.

defines which version of the surface char combustion law (Law ) is being used. If you want to use

the default diffusion-limited rate model, retain the selection of diffusion-limited in the drop-down

list. No additional inputs are necessary, because the binary diffusivity defined above will be used in

To use the kinetics/diffusion-limited rate model for the surface combustion model, select kin-

etics/diffusion-limited in the drop-down list and enter the parameters in the resulting Kinet-

ics/Diffusion-Limited Combustion Model Dialog Box (p. ).

To use the intrinsic model for the surface combustion model, select intrinsic-model in the

drop-down list and enter the parameters in the resulting Intrinsic Combustion Model Dialog

Box (p. ).

To use the multiple surface reactions model, select multiple-surface-reactions in the drop-

down list.

Pure Solvent Melting Heat

specifies the latent heat for the melting and solidification model (  in Equation . in the Theory

Guide).

specifies the solidus temperature for the melting and solidification model (

in the Theory Guide). If you are solving for species transport, the solidus temperature is

in

Equation ., and you specify the method by which it is calculated: either according to the mixing-

in

law (which is based on the parameters of the solutes) or a user-defined function.

specifies the liquidus temperature for the melting and solidification model (

in the Theory Guide). If you are solving for species transport, the liquidus temperature is

in

Pure Solvent Melting Temperature

specifies the melting temperature of pure solvent (

in Equation . and Equation . in the

Theory Guide) for the melting and solidification model when species transport has also been enabled.

The solvent is the last species listed under of the mixture material.

Eutectic Temperature

is the lowest alloy melting temperature, which depends on the relative proportions of the mixture

composition of the Eutectic species mass fractions.

Slope of Liquidus Line

specifies the slope of the liquidus surface with respect to the concentration of the solute (

in

Equation . and Equation . in the Theory Guide). It is not necessary to specify this value for the

solvent. Note that this option is available only for the melting and solidification model when species

transport has also been enabled.

Partition Coefficient

specifies the partition coefficient with respect to the concentration of the solute fluid (

in Equa-

tion . and Equation . in the Theory Guide). It is not necessary to specify this value for the solvent.

in Equa-

Note that this option is available only for the melting and solidification model when species transport

has also been enabled.

Eutectic Mass Fraction

is the mass fraction of a solute in an alloy at which the melting temperature of the alloy is the lowest

possible value (

in Equation . in the Theory Guide). It is not necessary to specify this value

for the solvent. Note that this option is available only for the melting and solidification model when

species transport has also been enabled.

Solutal Expansion Coefficient

allows you to specify the coefficient in Equation . in the Theory Guide for all the species except

the last one in the mixture. Note that this option is available only for the melting and solidification

model when the Include Solutal Buoyancy option is enabled.

Diffusion in Solid

specifies the rate of diffusion in the solid. Note that this option is available only for the melting and

solidification model when the Lever rule is selected and the species transport is enabled.

UDS Diffusivity

specifies the diffusion coefficient for a user-defined scalar.This material property is available in the

Create/Edit Materials Dialog Box (p. ) when you specify one or more user-defined scalars in the

User-Defined Scalars Dialog Box (p. ). If you select defined-per-uds, you will need to specify the

diffusion coefficient for each user-defined scalar transport equation in the UDS Diffusion Coefficients

Youngs Modulus

specifies the Young's modulus.This material property is only available for solid materials when you

have selected a model in the Structural Model Dialog Box (p. ).

Poisson Ratio

specifies the Poisson's ratio.This material property is only available for solid materials when you have

selected a model in the Structural Model Dialog Box (p. ).

sets the material electrical conductivity.You may set a constant value, or select one of the other

methods from the drop-down list above the real number field.This material property only becomes

available if the electric potential model is enabled.

Charge Number

specifies the charge number for a fluid material for a flow involving electrochemical reactions.The

default setting of  means that the fluid species is neutral.This material property only becomes

When you are viewing the database, additional properties may be displayed. However, after you

copy the material to the local area, only the properties with relevance to the current problem will

changes the properties of a locally stored material or creates a new one in the local area. If no material

with the specified Name exists locally, ANSYS Fluent will create it. If you have modified the material

without changing its name, ANSYS Fluent will simply update the material with your modifications. If you

have assigned a new name to the material and a material with this name already exists locally, an error

will be indicated; you must then specify a different name or delete the existing material with that name

before trying to save the new material.

Delete

Delete

deletes the currently selected material from the local materials list. It has no effect on the global database.

The Fluent Database Materials dialog box is opened by clicking the Fluent Database... button in

the Create/Edit Materials Dialog Box (p. ). In this dialog box you can view the global (site-wide)

material properties database and copy materials list in the solver. See Copying Materials from the

ANSYS Fluent Database (p. ) for details.

Controls

contains a list of all materials of the selected Material Type that are defined in the database.The name

of this list will change depending on the selected material type (for example, fluid, solid, and so on).You

can select one or more of these materials to be copied to the solver.

Copy Materials from Case...

opens the Copy Case Material Dialog Box (p. ).

Delete

deletes the selected materials from the database.

contains fields for the material properties that are defined for the selected material.These fields are for

Delete

informational purposes only; they cannot be edited.

When you are viewing the database, not all properties displayed are relevant to your ANSYS Flu-

ent solution. After you copy the material, only properties with relevance to the current physical

models will be displayed.

Copy

copies the current material from the global database to the local materials list in the solver.

The Open Database dialog box is opened by clicking the User-Defined Database button in the Cre-

ate/Edit Materials Dialog Box (p. ).

Controls

Browse...

opens The Select File Dialog Box (p. ) where you can select the user-defined database to be used in

the current solver session.

Database Name

allows you to enter the path and name of a new database. If you select an existing database, this field

displays the path and name of the selected database.

The User-Defined Database Materials dialog box is opened by clicking OK in the Open Database

Dialog Box (p. ). In this dialog box you can view the user-defined material properties database and

copy materials list in the solver. See Viewing Materials in a User-Defined Database (p. ) for details.

Controls

User-Defined Materials

of this list will change depending on the selected material type (for example, User-Defined Fluid Mater-

ials, User-Defined Solid Materials, and so on).You can select one or more of these materials to copy to

your local list or edit their properties.

is a drop-down list containing all of the available material types.

Order Materials By

allows you to order the materials in the User-Defined Materials list alphabetically by Name or alphabet-

ically by Chemical Formula.

Delete

lists the properties and values of the selected material.

New...

opens a blank Material Properties Dialog Box (p. ) where you can define a new material.

Edit...

opens the Material Properties Dialog Box (p. ) displaying the properties of the selected material.

Save

saves the information to the selected database.

Copy

copies the selected material to your local material list. If the material already exists the New Material Name

Dialog Box (p. ) opens

This dialog box is opened by clicking the Copy Materials from Case... button in the User-Defined

Database Materials Dialog Box (p. ).

Controls

Case Materials

lists all the materials present in your local materials list.

Copy

copies the selected materials to the user-defined database.

This dialog box is opened by clicking New... button in the User-Defined Database Materials Dialog

Box (p. ). See Creating a New Materials Database and Materials (p. ) for details.

Controls

Name

specifies the name of the material that you are creating.

Formula

(optional) specifies the chemical formula of the material that you are creating.

Types

Controls

Name

Formula

Types

allows you to select material type from fluid, solid, inter-particle, droplet-particle, combusting-particle,

and mixture materials.

Available Properties

lists properties applicable to the selected material type.

Material Properties

lists properties that you have selected from Available Properties list.

Edit...

opens Edit Property Methods Dialog Box (p. ) where you can edit the parameters that define a property.

This dialog box is opened by clicking Edit... button in the Material Properties Dialog Box (p. ). See

Creating a New Materials Database and Materials (p. ) for details.

Controls

Property Name

specifies the name of the property that you want to edit.

specifies the methods that can be used to define the selected property.

Edit Properties

allows you to select the property that you want to edit.

This dialog box is opened by clicking the Copy button in the User-Defined Database Materials Dialog

Box (p. ) when a material is already defined with the same name in the Create/Edit Materials Dialog

Box (p. ).

Controls

New Name

allows you to enter the new name for the material you need to copy.

New Formula

allows you to enter the new formula for the material you need to copy.

The Polynomial Profile dialog box allows you to define a physical property as a polynomial function

of temperature. This dialog box will open when you select polynomial in the drop-down list next to

a physical property in the Create/Edit Materials Dialog Box (p. ). See Inputs for Polynomial Func-

tions (p. ) for details about the items below.

Controls

Define

shows the property that is being defined as a function of temperature.

In Terms of

shows the independent variable (Temperature).The property shown in Define will be defined as a

polynomial function of temperature.

is an integer number entry that indicates the number of coefficients to be defined.You can define up to

coefficients.

contains real number entries for the number of coefficients set in the Coefficients integer number

entry above.The number of entries that are editable will be the same as the number of coefficients you

requested.

The Piecewise-Linear Profile dialog box allows you to define a physical property as a piecewise-linear

function of temperature. This dialog box will open when you select piecewise-linear in the drop-down

list next to a physical property in the Create/Edit Materials Dialog Box (p. ). See Inputs for Piecewise-

Linear Functions (p. ) for details about the items below.

Controls

Define

In Terms of

piecewise-linear function of temperature.

Points

indicates the number of data pairs that will define the piecewise distribution.You can define up to

pairs.

Data Points

Points

pairs.

contains entries for defining the data pairs.

Point

indicates the point for which the data pair (Temperature, Value) is being defined.

is the independent variable.

Value

is the dependent variable (the property). In the example dialog box above, Viscosity is the variable

being defined, as shown in the Define field.

The Piecewise-Polynomial Profile dialog box allows you to define a physical property as a piecewise-

polynomial function of temperature. This dialog box will open when you select piecewise-polynomial

in the drop-down list next to a physical property in the Create/Edit Materials Dialog Box (p. ). See

Inputs for Piecewise-Polynomial Functions (p. ) for details about the items below.

Controls

Define

In Terms of

Ranges

sets the number of temperature ranges for which you will define polynomial functions.You can define

up to  ranges.

Range

indicates the temperature range for which you are defining the polynomial function.

Minimum, Maximum

set the minimum and maximum temperatures for the specified Range.

is an integer number entry that indicates the number of coefficients to be defined for the specified Range.

You can define up to  coefficients.

requested for the specified Range.

The Model Options dialog box allows you to select boiling model options and to enable the calculation

of the Spalding heat number for the convection/diffusion vaporization model. This dialog box opens

when you click Edit... next to Vaporization Model in the Create/Edit Materials Dialog Box (p. ).

Convection/Diffusion Vaporization Model

allows you to enable Variable Lewis Number Formulation if you want to compute the Spalding heat

number from Equation . in the Fluent Theory Guide.This group box is available only when you select

convection/diffusion-controlled for Vaporization/Boiling Model.

is where you can select the Use the Specific Heat of the Evaporating Species in Boiling Law option.

in Equation . in the Fluent Theory Guide) to the

specific heat of the evaporating species selected in the Set Injection Properties dialog box. For the

convection/diffusion controlled model with the Variable Lewis Number Formulation, this option is

selected by default.This ensures consistency with the convection/diffusion controlled model expression

for

For more information, see Description of the Properties (p. ).

The Compressible Liquid dialog box allows you to model liquid compressibility for high pressure

applications using the Tait equation of state. This dialog box will open when you select compressible-

liquid in the drop-down list next to one of the Properties in the Create/Edit Materials Dialog Box (p. ).

See Compressible Liquid Density Method (p. ) for details about using the items below.

Controls

sets the reference pressure.

sets the reference density.

sets the reference bulk modulus.

sets the density exponent.

The User-Defined Functions dialog box allows you to choose which user-defined function is to be

used to define a material property. This dialog box will open when you select user-defined in the

drop-down list next to one of the Properties in the Create/Edit Materials Dialog Box (p. ). See the

separate Fluent Customization Manual for details about user-defined functions.

The list will contain all available user-defined functions.

The Sutherland Law dialog box allows you to set the coefficients for Sutherland’s law for viscosity.

This dialog box will open when you select sutherland in the drop-down list next to Viscosity in the

Create/Edit Materials Dialog Box (p. ). See Sutherland Viscosity Law (p. ) for details about the

Controls

Methods

contains options for selecting the Two Coefficient Method or the Three Coefficient Method.

C1, C2

set the coefficients

and

in Equation . (p. ) in SI units.These inputs will appear if you select the

C1, C2

and

Two Coefficient Method.

Reference Viscosity

sets the reference viscosity

in Equation . (p. ).This input will appear if you select the Three

Coefficient Method.

sets the reference temperature

Effective Temperature

sets the effective temperature  in Equation . (p. ).This input will appear if you select the Three

The Power Law dialog box allows you to set the coefficients for the power law for viscosity. This dialog

box will open when you select power-law in the drop-down list next to Viscosity in the Create/Edit

Materials Dialog Box (p. ). See Power-Law Viscosity Law (p. ) for details about the items below.

Controls

Methods

B

sets the coefficient  in Equation . (p. ) in SI units.This input will appear if you select the Two

sets the temperature exponent  in Equation . (p. ) or Equation . (p. ), depending on your

Method selection. If you are using the Two Coefficient Method, this input must be in SI units.

The Non-Newtonian Power Law dialog box allows you to set the parameters for the non-Newtonian

power law for viscosity. This dialog box will open when you select non-newtonian-power-law in the

drop-down list next to Viscosity in the Create/Edit Materials Dialog Box (p. ). See Power Law for

Non-Newtonian Viscosity (p. ) for details about the items below.

Controls

Methods

allows you to select the type of dependency on the viscosity.

Shear Rate Dependent

is where the viscosity is dependent on the shear rate.

Shear Rate and Temperature Dependent

is where the viscosity is dependent on the shear rate and the temperature.

sets the consistency index  in Equation . (p. ).

sets the power-law index  in Equation . (p. ).

Minimum Viscosity Limit, Maximum Viscosity Limit

set the minimum and maximum viscosity limits.

sets the reference temperature.

Activation Energy/R, alpha

is the ratio of the activation energy to the thermodynamic constant  in Equation . (p. ).

The Carreau Model dialog box allows you to set the parameters for the non-Newtonian Carreau

model for viscosity. This dialog box will open when you select carreau in the drop-down list next to

Viscosity in the Create/Edit Materials Dialog Box (p. ). See The Carreau Model for Pseudo-

Plastics (p. ) for details about the items below.

Controls

Methods

Controls

Methods

Time Constant, lambda

sets the time constant  in Equation . (p. ).

Zero Shear Viscosity, Infinite Shear Viscosity

set the zero and infinite shear viscosity limits

and

Reference Temperature,T_alpha

The Cross Model dialog box allows you to set the parameters for the non-Newtonian Cross model for

viscosity. This dialog box will open when you select cross in the drop-down list next to Viscosity in

the Create/Edit Materials Dialog Box (p. ). See Cross Model (p. ) for details about the items below.

Controls

Methods

sets the zero shear viscosity limit

Time Constant

The Herschel-Bulkley dialog box allows you to set the parameters for the non-Newtonian Herschel-

Bulkley model for viscosity. This dialog box will open when you select herschel-bulkley in the drop-

down list next to Viscosity in the Create/Edit Materials Dialog Box (p. ). See Herschel-Bulkley Model

for Bingham Plastics (p. ) for details about the items below.

Controls

Methods

Yield Stress Threshold

sets the yield stress threshold

Critical Shear Rate

set the critical shear rate

The Biaxial Conductivity dialog box allows you to define a biaxial orthotropic thermal conductivity,

which is applicable to solid materials used for the wall shell conduction model. This dialog box will

open when you select biaxial in the drop-down list next to Thermal Conductivity in the Create/Edit

Materials Dialog Box (p. ). See Biaxial Thermal Conductivity (p. ) for details about the items below.

Controls

Planar Conductivity

specifies the conductivity within the shell (or solid) region.

Transverse Conductivity

specifies the conductivity normal to the surface of the solid region.

The Cylindrical Orthotropic Conductivity dialog box allows you to define an orthotropic thermal

conductivity in cylindrical coordinates. This dialog box will open when you select cyl-orthotropic in

the drop-down list next to Thermal Conductivity in the Create/Edit Materials Dialog Box (p. ). See

Cylindrical Orthotropic Thermal Conductivity (p. ) for details about the items below.

Controls

Axis Origin

allows you to specify the origin of the cylindrical coordinate system.

X,Y, Z

specify the X,Y, and (for 3D cases) Z coordinates.

Axis Direction

(3D only) allows you to specify the direction of the axis.

X,Y, Z

specify  against the direction of the axis.

Radial Conductivity

specifies the conductivity in the radial direction.

Tangential Conductivity

specifies the conductivity in the tangential direction.

Axial Conductivity

(3D only) specifies the conductivity in the axial direction.

The Orthotropic Conductivity dialog box allows you to define an orthotropic thermal conductivity

for a solid material, using principal directions that do not have to aligned with the global coordinate

system of the simulation. This dialog box will open when you select orthotropic in the drop-down

list next to Thermal Conductivity in the Create/Edit Materials Dialog Box (p. ). See Orthotropic

Thermal Conductivity (p. ) for details about the items below.

Controls

Direction  Components, Direction  Components

specify the directions

and

in Equation . (p. ) as X,Y,Z vectors. For 2D cases, only Direction

Components will appear.

Conductivity , Conductivity , Conductivity

specify

,

, and

in Equation . (p. ) as constant, polynomial, piecewise-linear, or

piecewise-polynomial functions of temperature. For 2D cases, only Conductivity  and Conductivity

will appear.

Edit...

opens the appropriate dialog box so you can enter a temperature-dependent conductivity. (This button

will be unavailable if you specify a constant conductivity.)

The Anisotropic Conduction - Principal Components dialog box allows you to define an anisotropic

thermal conductivity using the components of the principal axes (which do not have to be orthogonal

and/or aligned with the global coordinate system) and the associated principal values. This dialog box

will open when you select principal-axes-values in the drop-down list next to Thermal Conductivity

in the Create/Edit Materials Dialog Box (p. ). See Principal Axes and Principal Values (p. ) for details

about the items that follow.

Controls

specifies the , , and  components of the

,

, and

vectors (in Equation . (p. )) that define

the principal axes of the anisotropic material. Note that these vectors must be linearly independent.

Principal Values

specifies the principal values (

,

, and

,

, and

in Equation . (p. )) associated with the principal axes.

specifies the value of  (in Equation . (p. )) as a constant, function of temperature (polynomial,

piecewise-linear, piecewise-polynomial), or user-defined function.

Edit...

opens the appropriate dialog box for the definition of a temperature-dependent or user-defined conduct-

ivity. (This button will be unavailable if you specify a constant conductivity.)

The Anisotropic Conductivity dialog box allows you to define a general anisotropic thermal conduct-

ivity. This dialog box will open when you select anisotropic in the drop-down list next to Thermal

Conductivity in the Create/Edit Materials Dialog Box (p. ). See Anisotropic Thermal Conductiv-

ity (p. ) for details about the items below.

Controls

Matrix Components

specify the components of the matrix

specifies the value of  in Equation . (p. ) as a constant, function of temperature (polynomial,

Edit...

opens the appropriate dialog box so you can enter a temperature-dependent or user-defined conductivity.

(This button will be unavailable if you specify a constant conductivity.)

The Species dialog box (opened by clicking the Edit... button next to Mixture Species in the Create/Edit

Materials Dialog Box (p. ))) allows you to define the species that make up a mixture material. See

Defining the Species in the Mixture (p. ) for details about the items below.

(Note that the Species dialog box is a modal dialog box, which means that you must tend to it imme-

diately before continuing the property definitions.)

Controls

Mixture

shows the name of the mixture material for which you are defining the species.This field is not editable.

Available Materials

is a list of all of the materials to be a component in the mixture material by selecting it and clicking the

Add button below the Selected Species or Selected Surface Species list.To add a material to the

Available Materials list, use the Fluent Database Materials Dialog Box (p. ) to copy the fluid material

to local storage.

Selected Species

is a list of all the fluid-phase species in the mixture.You can modify the list as follows:

To add a material to the list, select it in the Available Materials list and click the Add button below

the Selected Species list.

To remove a material, select it in the Selected Species list and click Remove.

To move a bulk species to the bottom of the Selected Species list, select the species and click Last

Species.The transport equation will not be solved for the last species.

See Overview of the Species Dialog Box (p. ) for more information.

Selected Solid Species

is a list of all the solid species in the mixture.To add a material to the list, select it in the Available Mater-

ials list and click the Add button below the Selected Solid Species list.To remove a material, select it

in the Selected Solid Species list and click Remove. See Overview of the Species Dialog Box (p. ) for

Selected Site Species

is a list of all the site species in the mixture.To add a material to the list, select it in the Available Mater-

ials list and click the Add button below the Selected Site Species list.To remove a material, select it in

the Selected Site Species list and click Remove. See Overview of the Species Dialog Box (p. ) for more

The Reactions dialog box (opened by clicking the Edit... button next to Reaction in the Create/Edit

Materials Dialog Box (p. )) allows you to define the reactions for a mixture material. See Defining

Reactions (p. ) for details about using this dialog box.

(Note that the Reactions dialog box is a modal dialog box, which means that you must tend to it im-

mediately before continuing the property definitions.)

Controls

Mixture

Total Number of Reactions

sets the total number of reactions (fluid-phase reactions and surface reactions occurring at wall boundaries).

Use the arrows to change the value, or type in the value and press RETURN.

Reaction Name

contains the name of the reaction.

ID

sets the number of the reaction you want to define. (Again, if you type in the value be sure to press RE-

TURN.)

Reaction Type

contains options that allow you to specify the type of reaction.

specifies, if enabled, that the current reaction is a volumetric reaction.

specifies, if enabled, that the current reaction is a wall surface reaction.

specifies, if enabled, that the current reaction is a particle surface reaction.

Number of Reactants

indicates the number of reactants in the specified reaction.

Species

contains drop-down lists of all species in the mixture. (The number of lists will be equal to the Number

of Reactants.) Select each reactant in one of these lists.

specifies the stoichiometric coefficient of the reactant species in the reaction.

specifies the rate constant for the reactant species in the reaction.

Number of Products

indicates the number of products in the specified reaction.

Species

of Products.) Select each product in one of these lists.

specifies the stoichiometric coefficient of the product species in the reaction.

specifies the rate constant for the product species in the reaction.

contains inputs related to the Arrhenius rate. (If you have chosen Eddy-Dissipation for the Turbulence-

Chemistry Interaction in the Species Model Dialog Box (p. ), these inputs are not required.)

Guide, are mass/volume-time (for example, kg/

s).

Important

s).

Important

for

,

, and so on.

Include Backward Reaction

specifies that the reaction is reversible. By default, the backward reaction rate constant will be com-

puted from Equation . in the Fluent Theory Guide.You can specify your own backward reaction rate

parameters in the Backward Reaction Parameters Dialog Box (p. ). In this case, the backward reaction

rate constant will be computed from Equation . in the Fluent Theory Guide.

allows you to specify and use third-body efficiencies (

in Equation . in the Theory Guide).These

inputs are optional. (This item is available only if you have selected Volumetric for the Reaction

Type.)

enables the modeling of a pressure fall-off reaction. See Inputs for Reaction Definition (p. ) Finite-

Rate/No TCI or Eddy-Dissipation Concept for the Turbulence-Chemistry Interaction in the Species

Model Dialog Box (p. ) and have selected Volumetric for the Reaction Type.)

Coverage-Dependent Reaction

is used when modeling Wall Surface reactions with site-balancing and reaction rates depend on site

coverages.

Specify...

opens the Backward Reaction Parameters Dialog Box (p. ), Third-Body Efficiency Dialog Box (p. ),

the Pressure-Dependent Reaction Dialog Box (p. ), or Coverage-Dependent Reaction Dialog

Box (p. ) in which you can specify the backward rate parameters for the reversible reaction, third-

body efficiencies, pressure-dependent reaction parameters, or coverage parameters.

Mixing Rate

contains inputs related to the mixing rate. (If you have chosen Finite-Rate/No TCI or Eddy-Dissipation

Concept for the Turbulence-Chemistry Interaction in the Species Model Dialog Box (p. ), these inputs

are not required.)

A

is the constant  in the turbulent mixing rate (Equation . and Equation . in the Theory Guide)

when it is applied to a species that appears as a reactant in this reaction.The default setting of . is

based on the empirically derived values given by Magnussen and Hjertager [] (p. ).

B

is the constant  in the turbulent mixing rate (Equation . in the Theory Guide) when it is applied

to a species that appears as a product in this reaction.The default setting of . is based on the em-

pirically derived values given by Magnussen and Hjertager [] (p. ).

Particle Surface Reaction

contains inputs related to a particle surface reaction. See User Inputs for Particle Surface Reactions (p. )

for details. (This section will appear only if you have selected Particle Surface for the Reaction Type.)

Diffusion Limited Species

is a drop-down list that allows you to select the species for which the concentration gradient between

the bulk and the particle surface is the largest when there is more than one gaseous reactant taking

part in the particle surface reaction. See User Inputs for Particle Surface Reactions (p. ) for details.

Butler-Volmer/Tafel Parameters

contains inputs related to an electrochemical reaction. See User Inputs for Electrochemical Reactions (p. )

for details. (This group box appears only if Electrochemical is selected for Reaction Type.)

Tafel Parameters

indicates whether the Bulter-Volmer equation (Equation . in the Fluent Theory Guide) or the Tafel

equation (Equation . in the Fluent Theory Guide) is used in the kinetics calculation.

Anodic Transfer Coefficient

used in Equation . in the Fluent Theory Guide.This item appears if the Tafel

Parameters check box is cleared.

Cathodic Transfer Coefficient

Anodic Tafel Slope

in Equation . in the Fluent Theory Guide.This item appears only if the Tafel

Parameters check box is selected.

Cathodic Tafel Slope

Exchange Current Density

is the value of  used in Equation . in the Fluent Theory Guide

Equilibrium Potential

used in Equation . in the Fluent Theory Guide

Specify Reference Mass Fractions...

opens the Reference Mass Fractions Dialog Box (p. ).

The Backward Reaction Parameters dialog box (opened by clicking Specify... next to Include Back-

ward Reaction in the Reactions Dialog Box (p. )) allows you to specify your custom backward rate

parameters for a reversible reaction. See Inputs for Reaction Definition (p. ) for details.

Arrhenius Backward Rate

allows you to specify backward rate parameters.

in the backward rate constant expression in Equation . in the Fluent Theory Guide.

The Third-Body Efficiency dialog box (opened by clicking Specify... next to the Third-Body Efficiencies

button in the Reactions Dialog Box (p. )) allows you to specify the third-body efficiencies for each

species in the mixture, to be used in Equation . in the Theory Guide. See Defining Reactions (p. )

(Note that the Third-Body Efficiency dialog box is a modal dialog box, which means that you must

tend to it immediately before continuing the property definitions.)

Controls

Species

displays the name of each species in the mixture.

Third-body Efficiency

specifies the third-body efficiency for each species.

The Pressure-Dependent Reaction dialog box (opened by clicking Specify... under Pressure-Depend-

ent Reaction in the Reactions Dialog Box (p. )) allows you to specify parameters for a pressure fall-

off reaction. See Inputs for Reaction Definition (p. ) for details.

(Note that the Pressure-Dependent Reaction dialog box is a modal dialog box, which means that

you must tend to it immediately before continuing the property definitions.)

Controls

Reaction Parameters

contains inputs for specifying the type of pressure fall-off reaction and the reaction parameters. See

Pressure-Dependent Reactions in the Theory Guide for details.

contains a drop-down list of the available reaction types: lindemann, troe, and sri. See Pressure-De-

pendent Reactions in the Theory Guide for details.

Bath Gas Concentration

allows you to specify if the bath gas concentration (

in Equation . in the Theory Guide) is to

be defined as the concentration of the mixture, or as the concentration of one of the mixture’s con-

stituent species.

Chemically Activated Bimolecular Reaction

results in a net rate constant at any pressure being defined as Equation . in the Theory Guide.

Low Pressure Arrhenius Rate

contains inputs for specifying low-pressure Arrhenius parameters.

ln(Pre-exponential Factor)

is the natural logarithm of the constant

in Equation . in the Theory Guide.The pre-exponential

factor

is often an extremely large number, so you will enter the natural logarithm of this term.

Troe parameters

contains inputs for specifying parameters for the Troe method. See Pressure-Dependent Reactions in the

Theory Guide for details. (This section of the dialog box will appear only if you have selected troe as the

Reaction Type.)

Alpha

is the constant  in Equation . in the Theory Guide.

T1

T2

T3

SRI Parameters

contains inputs for specifying parameters for the SRI method. See Pressure-Dependent Reactions in the

Theory Guide for details. (This section of the dialog box will appear only if you have selected sri as the

a

b

c

d

e

The Coverage-Dependent Reaction dialog box (opened by clicking on Specify... under Coverage-

Dependent Reaction in the Reactions Dialog Box (p. )) allows you to model Wall Surface reactions

with site-balancing.

(Note that the Coverage-Dependent Reaction dialog box is a modal dialog box, which means that

Controls

Species

are the site species of the reaction.

Eta

is the surface coverage rate modification of the species and is defined in Equation . in the Theory

Guide.

Controls

Species

Eta

Guide.

Mu

Guide.

Eps

Guide.

The Reference Mass Fractions dialog box (opened by clicking Specify Reference Mass Fractions...

under Butler-Volmer/Tafel Parameters in the Reactions Dialog Box (p. )) allows you to specify

reference species mass fractions for the electrochemical reaction.

(Note that the Reference Mass Fractions dialog box is a modal dialog box, which means that you

must tend to it immediately before continuing the property definitions.)

Controls

Species

are the electrochemical reaction species used in the Butler-Volmer equation (Equation . in the Fluent

Reference Mass Fractions

contains inputs for the reference mass fractions of electrochemical reaction species (

The Reaction Mechanisms dialog box (opened by clicking the Edit... button next to Mechanism in

the Create/Edit Materials Dialog Box (p. )) allows you to select the reaction mechanism at a particular

zone. See Mixture Materials (p. ) for details about these methods and the related inputs.

(Note that the Reaction Mechanisms dialog box is a modal dialog box, which means that you must

Controls

Number of Mechanisms

specifies the number of mechanisms present.

Mechanism ID

Controls

is the ID of the mechanism that you specify.

Name

allows you to enter a name for the mechanism.

specifies the type of reaction to be displayed for the mechanism.

displays all volumetric reactions under the Reactions list.

displays all wall surface reactions under the Reactions list.

displays all particle surface reactions under the Reactions list.

displays all electrochemical reactions under the Reactions list.

All

displays all types of reactions under the Reactions list.

Reactions

displays the list of reactions of the category specified under Reaction Type.

Number of Sites

specifies the number of sites at which you can specify the reaction.

Site Name

contains the name of the site.

allows you to specify the site density of the species

Define...

opens the Site Parameters Dialog Box (p. ).

The Site Parameters dialog box (opened by clicking the Define... button next to Site Density in the

Reaction Mechanisms Dialog Box (p. )) allows you to define the coverage for each site species.

Controls

Site Name

displays the name of site.

specifies the total number of site species.

Site Species

allows you to select the site species.

Initial Site Coverage

allows you to specify the initial coverage of the site species.

The Mass Diffusion Coefficients dialog box (opened by clicking the Edit... button next to Mass Dif-

fusivity in the Create/Edit Materials Dialog Box (p. ) allows you to define the diffusion coefficients

of the species in the mixture. Its contents will depend on the method you selected for Mass Diffusivity.

See Mass Diffusion Coefficient Inputs (p. ) for details about these methods and the related inputs.

(Note that the Mass Diffusion Coefficients dialog box is a modal dialog box, which means that you

For the dilute-approx method:

Controls

Species Di

contains a selectable list of all species in the mixture, from which you can select each species and specify

its diffusion coefficient.

sets the diffusion coefficient for the selected species in the mixture.

For the multicomponent method:

Controls

Species Di, Species Dj

contain selectable lists of species in the mixture, from which you can select each pair of species and

specify the diffusion coefficient of the selected Species Di in the selected Species Dj.

sets the diffusion coefficient for Species Di in Species Dj (which is equivalent to the diffusion coefficient

for Species Dj in Species Di).

The Thermal Diffusion Coefficients dialog box (opened by clicking the Edit... button next to Thermal

Diffusion Coefficient in the Create/Edit Materials Dialog Box (p. ) allows you to define the thermal

diffusion coefficients of the species in the mixture. See Thermal Diffusion Coefficient Inputs (p. ) for

details about these methods and the related inputs.

(Note that the Thermal Diffusion Coefficients dialog box is a modal dialog box, which means that

Controls

Species Thermal Di

its thermal diffusion coefficient.

sets the thermal diffusion coefficient for the selected species in the mixture.

The UDS Diffusion Coefficients dialog box (opened by selecting uds and clicking the Edit... button

next to UDS Diffusivity in the Create/Edit Materials Dialog Box (p. )) allows you to define the diffusion

coefficients for your user-defined scalar transport equations.

(Note that the UDS Diffusion Coefficients dialog box is a modal dialog box, which means that you

Controls

User-Defined Scalar Diffusion

contains a selectable list of all user-defined scalars, from which you can select each one and specify its

sets the diffusion coefficient for the selected user-defined scalar.

The WSGGM User Specified dialog box opens when you select wsggm-user-specified as the input

method for a composition-dependent Absorption Coefficient in the Create/Edit Materials Dialog

Box (p. ) and it allows you to define the path length for he weighted-sum-of-gray-gases model. See

Inputs for a Composition-Dependent Absorption Coefficient (p. ) for details.

Controls

Path Length

allows you to set the Path Length equal to a mean beam length that you have calculated outside of

Fluent.

The Gray-Band Absorption Coefficient allows you to specify a different absorption coefficient in each

gray band when you are modeling non-gray radiation with the P-, DO, or MC models (see The P-

Model Equations, The DO Model Equations, or Monte Carlo (MC) Radiation Model Theory in the Theory

Guide and Setting Up the P- Model with Non-Gray Radiation (p. ), Defining Non-Gray Radiation for

the DO Model (p. ), or Setting Up the MC Model (p. )). This dialog box will open when you select

gray-band in the drop-down list next to Absorption Coefficient in the Create/Edit Materials Dialog

Box (p. ).

Controls

band n

specifies the absorption coefficient for the

th gray band.

The Delta-Eddington Scattering Function dialog box allows you to define the parameters used in

the Delta-Eddington phase function for radiation scattering. This dialog box will open when you select

delta-eddington in the drop-down list next to Scattering Phase Function in the Create/Edit Materials

Dialog Box (p. ). See Anisotropic Scattering for details about the items below.

Controls

Forward Scattering Factor

Asymmetry Factor

The Gray-Band Refractive Index allows you to specify a different refractive index in each gray band

when you are modeling non-gray radiation with the P-, DO, or MC model (see The P- Model Equations,

The DO Model Equations, or Monte Carlo (MC) Radiation Model Theory in the Theory Guide and Setting

Up the P- Model with Non-Gray Radiation (p. ), Defining Non-Gray Radiation for the DO Model (p. ),

or Setting Up the MC Model (p. )). This dialog box will open when you select refractive-band in

the drop-down list next to Refractive Index in the Create/Edit Materials Dialog Box (p. ).

Controls

Band n

specifies the refractive index for the

The Single Rate Model dialog box (which opens when you select single-rate from either the Devo-

latilization or Themolysis Model drop-down list in the Create/Edit Materials Dialog Box (p. )) allows

you to specify the parameters used in either the single kinetic rate devolatilization model or single

kinetic rate Thermolysis model. For more details about these models, see Devolatilization (Law ) and

Mass Transfer During Law —Thermolysis in the Fluent Theory Guide, respectively.

Note that the Single Rate Model dialog box is a modal dialog box, which means that you must tend

to it immediately before continuing the property definitions.

Controls

sets the value of:

Devolatilization model:

in Equation . in the Theory Guide for the computation of the kinetic

rate.

Thermolysis model:

in Equation . (for droplet particles) or

rate.

Theory Guide (for multicomponent particles).

rate.

The Two Competing Rates Model dialog box (which opens when you select two-competing-rates

as the Devolatilization Model in the Create/Edit Materials Dialog Box (p. ) allows you to specify

the parameters used for each of the competing rates in the two-competing-rates devolatilization

model. See Devolatilization (Law ) in the Theory Guide for details.

Note that the Two Competing Rates Model dialog box is a modal dialog box, which means that you

must tend to it immediately before continuing the property definitions.

Controls

First Rate

sets parameters for the first of the two rates.

Weighting Factor

Second Rate

sets parameters for the second of the two rates.

The CPD Model dialog box (which opens when you select cpd-model as the Devolatilization Model

in the Create/Edit Materials Dialog Box (p. )) allows you to specify the parameters used in the CPD

devolatilization model. See Devolatilization (Law ) in the Theory Guide for details.

Note that the CPD Model dialog box is a modal dialog box, which means that you must tend to it

immediately before continuing the property definitions.

Controls

Initial Fraction of Bridges in Coal Lattice

Initial Fraction of Char Bridges

Lattice Coordination Number

Cluster Molecular Weight

Side Chain Molecular Weight

The Kinetics/Diffusion-Limited Combustion Model dialog box (which opens when you select kinet-

ics/diffusion-limited as the Combustion Model in the Create/Edit Materials Dialog Box (p. ) allows

you to specify the parameters used for the kinetics/diffusion-limited rate surface combustion model.

See Surface Combustion (Law ) in the Theory Guide for details.

Note that the Kinetics/Diffusion-Limited Combustion Model dialog box is a modal dialog box, which

means that you must tend to it immediately before continuing the property definitions.

Controls

Controls

Mass Diffusion-Limited Rate Constant

sets the value for

Kinetics-Limited Rate Pre-exponential Factor

Kinetics-Limited Rate Activation Energy

sets the value for  in Equation . in the Theory Guide.

The Intrinsic Combustion Model dialog box (which opens when you select intrinsic-model as the

Combustion Model in the Create/Edit Materials Dialog Box (p. ) allows you to specify the parameters

used for the intrinsic surface combustion model. See Surface Combustion (Law ) in the Theory Guide

Note that the Intrinsic Combustion Model dialog box is a modal dialog box, which means that you

Controls

Char Porosity

Mean Pore Radius

Specific Internal Surface Area

in Equation . and Equation . in the Theory Guide.

Tortuosity

Burning Mode, alpha

The Multiple Surface Reactions dialog box (which opens when you select multiple-surface-reactions

as the Combustion Model in the Create/Edit Materials Dialog Box (p. )) allows you to enable com-

position-dependent char properties when using the multiple surface reactions combustion model.

Controls

enables calculation of the char specific heat from the particle specific heat values. See Combustion

Model

(p. ) for details.

enables calculation of the char density from the particle density values. See Combustion Model

(p. )

The Edit Material dialog box contains the portion of the Create/Edit Materials Dialog Box (p. ) that

contains the properties for a specific material. It is opened from the Primary Phase Dialog Box (p. ),

Secondary Phase Dialog Box (p. ), Wall Dialog Box (p. ), Fluid Dialog Box (p. ), or Solid Dialog

Box (p. ).

Controls

Properties of material-n

contains a list of the properties of material- .The items in the list are the same as those in the Create/Edit

Change

applies any changes you have made to the properties of the material.

.. Phases

The Phases dialog box allows you to define each of the phases and the interaction between them. See

– Defining the Phases for the Eulerian Model (p. ) for details.

Controls

Phases

contains a list of all of the phases in the problem from which you can select the phase you want to define

or modify. A phase can be a Primary Phase or a Secondary Phase.You cannot change a phase from

primary to secondary, or vice versa. Instead, you can redefine the properties of the primary phase to reflect

the new phase designated as primary, and redefine the secondary phases accordingly as well.

Edit...

opens either the Primary Phase Dialog Box (p. ) or the Secondary Phase Dialog Box (p. ), where you

can define the properties of the selected primary or secondary phase.

Phases

Interaction...

opens the Phase Interaction Dialog Box (p. ), where you can define the interaction between the phases

(for example, surface tension if you are using the VOF model, slip velocity functions if you are using the

mixture model, or drag functions if you are using the Eulerian model).

ID

displays the ID number of the phase.You will need this number only if you are writing a user-defined

function. See the separate Fluent Customization Manual for details about writing user-defined functions

for multiphase applications.

... Primary Phase Dialog Box

... Secondary Phase Dialog Box

... Discrete Phase Dialog Box

... Phase Interaction Dialog Box

The Primary Phase dialog box allows you to set the properties of the primary phase. It is opened from

the Phases (p. ). See Defining the Phases for the VOF Model (p. ) for details about the items below.

Controls

Name

specifies the name of the phase.

Phase Material

contains a drop-down list of available materials, from which you can select the appropriate one for this

phase.

Edit...

opens the Edit Material Dialog Box (p. ) for the selected Phase Material, where you can modify its

phase.

Edit...

The Secondary Phase dialog box allows you to set the properties of a secondary phase. It is opened

from the Phases (p. ). The items that appear in the Secondary Phase dialog box will depend on

which multiphase model you are using. See Defining the Phases for the VOF Model (p. ), Defining

the Phases for the Mixture Model (p. ), and Defining the Phases for the Eulerian Model (p. ) for

details about the items below.

Controls

Name

contains a drop-down list of available materials, from which you can select the appropriate one for the

phase.

Edit...

Granular

indicates whether or not this is a solid phase.This item appears only for the Eulerian model.

Phases

Packed Bed

indicates whether or not the granular phase is a packed bed.This option appears only if Granular is en-

abled.

Granular Temperature Model

lists the granular temperature models.

Phase Property

enables phase property model for granular temperature.

Partial Differential Equation

enables partial differential equation model for granular temperature. See Granular Temperature in

the Theory Guide for details.

is used to predict mass, momentum and energy transfers through the interface between the phases. See

Interfacial Area Concentration in the Theory Guide for details.

contains a list of phase-specific properties.This section of the dialog box will not appear for the VOF

model.The Diameter appears for both the mixture model and the Eulerian model, but all of the others

will appear only for a granular phase with the Eulerian model.

Diameter

constant value, or select user-defined to use a user-defined function. See the separate Fluent Cus-

tomization Manual for details about user-defined functions.

specifies the kinetic part of the granular viscosity of the particles (

Theory Guide).You can select constant (the default) in the drop-down list and specify a constant

value, select syamlal-obrien to compute the value using Equation . in the Theory Guide, select

gidaspow to compute the value using Equation . in the Theory Guide, or select user-defined

to use a user-defined function. Note that if you select user-defined, your user-defined function must

include both the kinetic portion and the collisional portion of the viscosity in the value it returns.

Angle Of Internal Friction

none to exclude frictional pressure from your calculation, johnson-et-al to apply Equation . in

the Theory Guide, syamlal-et-al to apply Equation . in the Theory Guide, based-ktgf, where

the frictional pressure is defined by the kinetic theory  [] (p. ).The solids pressure tends to a large

value near the packing limit, depending on the model selected for the radial distribution function.

You must hook a user-defined function when selecting the user-defined option. See the separate

can be set as derived, or as a user-defined function.This is defined as Equation . (p. ).

value is ..

specifies the solids conductivity.You can select syamlal-obrien, gidaspow, constant or user-defined.

value is ..

motion of the particles.You can choose the algebraic, constant, dpm-averaged,or user-defined

option. dpm-averaged is available only when using the Dense Discrete Phase Model (DDPM).

the arastapour, or a user-defined option.

(.)

with

.

specifies the maximum volume fraction for the granular phase. For monodispersed spheres the

specifies the attractive forces between the interfaces.

Phases

Coalescence Kernel

allows you to specify the coalescence kernel.You can select none, constant, hibiki-ishii, ishii-kim,

yao-morel, or user-defined.The three options, hibiki-ishii, ishii-kim, and yao-morel are described

in detail in Interfacial Area Concentration in the Theory Guide.

allows you to specify the breakage kernel.You can select none, constant, hibiki-ishii, ishii-kim, yao-

morel, or user-defined.The three options, hibiki-ishii, ishii-kim, and yao-morel are described in

detail in Interfacial Area Concentration in the Theory Guide.

phase.You can choose from constant or user-defined. If the Boiling Model option is enabled when

using the Eulerian multiphase model, you can also select yao-morel.The yao-morel option is described

in Yao-Morel Model in the Theory Guide.

will need to be specified if you selected yao-morel for the Breakage Kernel.

ishii and ishii-kim models.You can choose constant, wu-ishii-kim, fluent-ke, and user-defined for

the dissipation function.

is the value used in Equation . (p. ).This is available when the wu-ishii-kim formulation is se-

lected as the Dissipation Function.

Delete

deletes this phase.

The Discrete Phase dialog box allows you to set the properties of a discrete phase. It is opened from

the Phases (p. ). The items will appear in the Discrete Phase dialog box when the Dense Discrete

Phase Model option is enabled in the Multiphase Model dialog box. See Including the Dense Discrete

Phase Model (p. ) for details about the items below.

Controls

Name

Volume Fraction Approaching Continuous Flow Limit

appears for non-granular flows.When this option is enabled, only the Transition Factor must be specified.

Volume Fraction Approaching Packing Limit

prevents the unlimited accumulation of particles, which are operating at packing limit conditions.

Granular

Phases

contains a list of phase-specific properties.

to use a user-defined function.

the Theory Guide, syamlal-obrien to apply Equation . in the Theory Guide, based-ktgf, where

value is ..

value is ..

specifies the solids conductivity.You can select syamlal-obrien, gidaspow,or user-defined.

(.)

with

.

Transition Factor

is specified as either a constant or a user-defined function.The default value is assumed to be .,

which corresponds to the closest sphere packing for monosized spheres (a factor of /). In other

words, the transition criterion is based on the local particle volume fraction of the given discrete

phase and is specified as a factor multiplied by the maximum packing limit (also a user specified

value).

The Phase Interaction dialog box allows you to define the interaction between phases. It is opened

value).

from the Phases (p. ). The items that appear in the Phase Interaction dialog box will depend on

Controls

Virtual Mass

displays the Virtual Mass Coefficient inputs.This tab is active only for the Eulerian models.

Phases

Virtual Mass Modeling

includes the “virtual mass force” (

in Equation . in the Theory Guide) that is present when a

secondary phase accelerates relative to the primary phase.

Implicit

enables the implicit method for the virtual mass force which can improve convergence in some cases.

Virtual Mass Implicit Options

specifies what form of the implicit method to use. Default models the entire virtual mass force while

Option  and Option  model truncated expressions which may further improve convergence.

Virtual Mass Coefficient

specifies the virtual mass coefficient for each pair of phases. See Including the Virtual Mass Force (p. )

Drag

displays the Drag Coefficient inputs.This tab is active only for the Eulerian and mixture models.

Drag Coefficient

specifies the drag function for each pair of phases.This section of the dialog box appears only for the

Eulerian and mixture models. See Defining the Phases for the Eulerian Model (p. ) for information

about the available options.

Drag Modification

enables modification of the selected drag models by a drag factor and expands the dialog box

to show the Drag Factor settings. See Drag Modification (p. ) for additional information on

using Drag Modification.

Drag Factor

specifies the drag factor to use for modifying the specified drag model. See Drag Modifica-

tion (p. ) for additional information on specifying the Drag Factor.

Lift

displays the Lift Coefficient inputs.This tab is active only for the Eulerian model.

Lift Coefficient

specifies the lift function for each pair of phases.This section of the dialog box appears only for the

Eulerian model. See Defining the Phases for the Eulerian Model (p. ) for information about the

available options.

Wall Lubrication

displays the Wall Lubrication inputs. This tab is active only for the Eulerian model.

specifies the wall lubrication model for each primary-secondary phase pair.This section of the dialog

box appears only for the Eulerian model. See Including the Wall Lubrication Force (p. ) for inform-

ation about the available options.

Turbulent Dispersion

displays the Turbulent Dispersion inputs. This tab is active only for the Eulerian model.

specifies the turbulent dispersion model for each primary-secondary phase pair.This section of the

dialog box appears only for the Eulerian model. See Including the Turbulent Dispersion Force (p. )

for information about the available options.

Turbulence Interaction

displays the Turbulence Interaction inputs. This tab is active only for the Eulerian model.

specifies the turbulence interaction model for each primary-secondary phase pair.This section of the

dialog box appears only for the Eulerian model. See Including Turbulence Interaction Source

Terms (p. ) for information about the available options.

Collisions

displays the Restitution Coefficient inputs.

Restitution Coefficient

specifies the restitution coefficient for collisions between each pair of granular phases, and for collisions

between particles of the same granular phase. It is relevant only if two or more granular phases are

involved. See Defining the Phases for the Eulerian Model (p. ) for information about the available

options.

Slip

displays the Slip Velocity inputs.This tab is active only for the mixture model.

specifies the slip velocity function for each secondary phase with respect to the primary phase. See

Defining the Phases for the Mixture Model (p. ) for information about the available options.

Heat

displays the Heat Transfer Coefficient inputs.This tab is active only for the Eulerian model when the

energy equation is active.

specifies the heat transfer coefficient function between each pair of phases. See Including Heat

Transfer Effects (p. ) for information about the available options.

Mass

displays the Mass Transfer Function inputs.

Number of Mass Transfer Mechanisms

specifies the number of mass transfer mechanisms in your simulation. See Including Mass Transfer

Effects (p. ) for information about the available options.

Reactions

allows you to define multiple heterogeneous reactions and stoichiometry.

Total Number of Heterogeneous Reactions

specifies the total number of reactions (volumetric reactions, wall surface reactions, and particle surface

reactions). See Specifying Heterogeneous Reactions (p. ) for information about the available options.

Heterogeneous Stiff Chemistry Solver

is used in inter-phase reaction mechanisms containing numerically stiff reactions.This option can

improve convergence and is available for transient Eulerian multiphase simulations.

Phases

allows you to enter a name for the reaction.

ID

enables you to set the reaction ID for each reaction.

allows you to specify the number of reactants that are involved in the reaction.

allows you to specify the number of products that are involved in the reaction.

Phase

drop-down list allows you to select the phase that is involved in the reaction.

Species

drop-down list allows you to select the species.

allows you to set the stoichiometric coefficient.

Reaction Rate Function

allows you to choose rate exponents for an Arrhenius-type reaction, a user-defined function, or a

population balance mechanism for the reaction rate.

includes the effects of surface tension along the fluid-fluid interface.

Model

contains two surface tension models from which to choose.

Continuum Surface Force

adds the surface tension to the VOF calculation, which results in a source term in the momentum

equation.This method is available only for the VOF and Eulerian models.

Continuum Surface Stress

is an alternative way to modeling surface tension in a conservative manner compared to the

continuum surface force method.This method is available only for the VOF and Eulerian models.

Adhesion Options

contains options to include wall and jump adhesion.

Wall Adhesion

enables the specification of a wall adhesion angle. (The angle itself, as defined in Figure . : Meas-

uring the Contact Angle (p. ), will be specified in the Wall Dialog Box (p. ).)

Jump Adhesion

enables the treatment of the contact angle specification at the porous jump boundary. (The angle

itself will be specified in the Porous Jump Dialog Box (p. ).)

Surface Tension Coefficients

specify the surface tension coefficient,

in Equation . and Equation . in the Theory Guide,

for each pair of phases. See Defining the Phases for the VOF Model (p. ) for details.

allows you to use the diffusive and anti-diffusive discretization procedure across the distinct interfaces.

Phase Localized Compressive Scheme

enables the compressive discretization scheme in ANSYS Fluent, where the degree of diffusion/sharp-

ness is controlled through the value of the slope limiters.This item will appear only for the VOF

model and for the Eulerian model with Multi-Fluid VOF Model enabled.

Slope Limiters

are values equating to specific discretization schemes. For each pair of phases, you can enter a value

of , , or , or any value between  and . Depending on the value you use, first order upwind, second

order upwind, compressive, or the blended scheme will be applied. Refer to Table . : Slope Limiter

Discretization Scheme (p. ) to equate each value of the slope limiter with a discretization scheme.

For more information, refer to Discretizing Using the Phase Localized Compressive Scheme (p. ).

Interfacial Area

displays the Interfacial Area inputs.This tab appears only for the Mixture multiphase model with interphase

mass transfer and the Eulerian multiphase model. See Defining the Algebraic Interfacial Area Concentra-

tion (p. ) and Using an Algebraic Interfacial Area Model (p. ) for information about the available

options.

Mod.Trans'on

displays the VOF-to-DPM Model Transition inputs.This tab is available only when a DPM injection is set

as described in Setting up the VOF-to-DPM Model Transition (p. ).

Number of Model Transition Mechanisms

specifies the number of VOF-to-DPM model transition mechanisms in your simulation. See Setting

up the VOF-to-DPM Model Transition (p. ) for information about the available options.

The Cell Zones Conditions task page allows you to set the type of a cell zone and display other dialog

boxes to set the cell zone condition parameters for each zone. See Cell Zone Conditions (p. ) for

Cell Zone Conditions Task Page

Controls

Zone

contains a selectable list of available cell zones from which you can select the zone of interest.You can

check a zone type by using the mouse probe (see Controlling the Mouse Button Functions (p. )) on the

displayed physical mesh.This feature is particularly useful if you are setting up a problem for the first time,

or if you have two or more cell zones of the same type and you want to determine the cell zone IDs.To

do this you must first display the mesh with the Mesh Display Dialog Box (p. ).Then click the boundary

zone with the right (select) mouse button. ANSYS Fluent will print the cell zone ID and type of that

boundary zone in the console window.

Phase

specifies the phase for which conditions at the selected cell Zone are being set.This item appears if the

VOF, mixture, or Eulerian multiphase model is being used. See Defining Multiphase Cell Zone and Boundary

Conditions (p. ) for details.

Type

contains a drop-down list of condition types for the selected cell zone.The list contains all possible types

to which the cell zone can be changed.

ID

displays the cell zone ID number of the selected cell zone. (This is for informational purposes only; you

cannot edit this number.)

Edit...

opens the Fluid Dialog Box (p. ) or Solid Dialog Box (p. ).

Copy...

opens the Copy Conditions Dialog Box (p. ), which allows you to copy conditions from one cell zone to

other cell zones of the same type. See Copying Cell Zone and Boundary Conditions (p. ) for details.

Profiles...

opens the Profiles Dialog Box (p. ).

Parameters...

opens the Parameters Dialog Box (p. ).

Operating Conditions...

opens the Operating Conditions Dialog Box (p. ).

Display Mesh...

Porous Formulation

contains options for setting the velocity in the porous medium simulation. See Defining the Porous Velocity

Formulation (p. ) for details.

Superficial Velocity

enables the superficial velocity in a porous medium simulation.This is the default method.

Physical Velocity

enables the physical velocity in a porous medium simulation for a more accurate simulation.This option

is available only for a pressure-based solver. See Modeling Porous Media Based on Physical Velo-

city (p. ) for details.

... Fluid Dialog Box

... Solid Dialog Box

... Copy Conditions Dialog Box

... Operating Conditions Dialog Box

... Select Input Parameter Dialog Box

... Profiles Dialog Box

... Replicate Profile Dialog Box

... Orient Profile Dialog Box

...Write Profile Dialog Box

The Fluid dialog box sets the conditions for a fluid cell zone. It is opened from the Cell Zone Conditions

Task Page (p. ). See Inputs for Fluid Zones (p. ) and User Inputs for Porous Media (p. ) for details

about the items below.

Controls

Zone Name

sets the name of the zone.

Material Name

sets the fluid material.The drop-down list contains the names of all materials that have been loaded into

the solver. Materials are defined with the Materials Task Page (p. ).

Important

If you are modeling species transport or multiphase flow, the Material Name list will

not appear in the Fluid dialog box. For species calculations, the mixture material for all

fluid zones will be the material you specified in the Species Model Dialog Box (p. ).

For multiphase flows, the materials are specified when you define the phases, as de-

scribed in Defining the Phases for the VOF Model (p. ).

Frame Motion

enables the moving reference frame model for the cell zone. See Specifying the Rotation Axis (p. ) and

Defining Zone Motion (p. ) for details.

Mesh Motion

enables the sliding mesh model for the cell zone. See Setting Up the Sliding Mesh Problem (p. ) for

details.

Porous Zone

indicates that the zone is a porous medium. Additional items will appear in the dialog box when this

details.

option is enabled. See User Inputs for Porous Media (p. ) for details.

3D Fan Zone

allows you to simulate the effect of an axial fan by applying a distributed momentum source in a toroid-

shaped fluid volume.This model can calculate not only the axial velocity, but the swirl and radial velocities

as well.When you enable this option, the 3D Fan Zone tab becomes available, so that you can specify

the geometry and properties of the fan.The cell zone should have a toroid shape that is sized to match

the blade-swept volume of the fan you are simulating (that is, has an inner and outer radius that matches

the radius of the fan’s hub and blade tips, respectively, as well as a length that matches the thickness of

the toroid region swept by the blades in the axial direction). Furthermore, the fluid cell zone should be

“interior”, that is, have at least two boundary zones of type interior that border another fluid cell zone

and act as the fan inlet and outlet (the other boundaries can be of type interior as well). See 3D Fan

Laminar Zone

disables the calculation of turbulence production in the fluid zone (appears only for turbulent flow calcu-

lations using the Spalart-Allmaras model or one of the -  or -

models). See Specifying a Laminar

Zone (p. ) for details.

LES Zone

allows you to model a smaller embedded LES zone within a larger URANS computational domain for

turbulent flow calculations.When you turn on this option, the Embedded LES tab will be enabled to allow

you to specify properties for the embedded LES zone. See Setting Up the Embedded Large Eddy Simulation

(ELES) Model (p. ) for details.

enables the specification of volumetric sources of mass, momentum, energy, and so on.When you turn

on this option, the Source Terms tab will be enabled to allow you to specify the values for the desired

sources. See Defining Mass, Momentum, Energy, and Other Sources (p. ) for details.

Fixed Values

enables the fixing of the value of one or more variables in the fluid zone, rather than computing them

during the calculation. See Fixing the Values of Variables (p. ) for details.

Important

You can fix values for velocity components, temperature, and species mass fractions

only if you are using the pressure-based solver.

Participates In Radiation

specifies whether or not the fluid zone participates in radiation.This option appears when you are using

the DO model for radiation.

Warning

In general, disabling Participates in Radiation for fluid zones is not recommended, as

it can produce erroneous results. There are rare cases when it is acceptable: for example,

if the domain contains multiple fluid zones, disabling this option for zones where radi-

ation is negligible may save computational time without affecting the results.

Reaction

enables/disables reactions in the porous zone.

Electrolyte

indicates that the zone is an electrolyte zone. By default, all fluid zones are assumed to be electrolyte

zones.This option appears when the Electrochemical Reaction model is enabled.

lists the parameters that define motion for a moving reference frame.

Rotation-Axis Origin

specifies the origin for the axis of rotation of solid zone. See Specifying the Rotation Axis (p. ) for

details.This item will appear only for 3D and 2D non-axisymmetric models.

Rotation-Axis Direction

specifies the direction vector for the solid zone’s axis of rotation. See Specifying the Rotation Axis (p. )

for details.This item will appear only for 3D models.

Rotational Velocity

contains an input field for the rotational Speed of the zone.

Translational Velocity

contains inputs for the X, Y, and Z velocities of the zone.

Relative Specification

indicates whether the velocities are absolute velocities (absolute) or velocities relative to the motion

of each cell zone (Relative to Cell Zone).This selection is necessary only if your problem involves

moving reference frames or sliding meshes. If there is no zone motion, both options are equivalent.

UDF

allows you to hook the DEFINE_ZONE_MOTION user-defined function.

Copy to Mesh Motion

allows you to switch between the MRF and moving mesh models.The variables used for the origin,

axis, and velocity components, as well as for the DEFINE_ZONE_MOTION user-defined function, will

be copied from one model to the other.

UDF

Copy to Frame Motion

lists the parameters associated with the porous zone.

Conical

enables the specification of a conical (or cylindrical) porous medium.This item will appear only when

the Porous Zone option is enabled for a 3D case.

Cone Half Angle

specifies the angle between the cone’s axis and its surface (see Figure . : Cone Half Angle (p. )).

Set this to  to define the porous region using a cylindrical coordinate system.This item will appear

only when the Porous Zone and Conical options are enabled.

Snap to Zone

aligns the plane (or line, in 2D) tool with the zone selected in the drop-down list.The tool is centered

at the centroid of the zone, with the tool’s axis normal to the zone. If this axis is not the desired cone

axis, reposition the tool (as described in Using the Plane Tool (p. )).When you are satisfied with

the axis, click the Update From Plane Tool (or Update From Line Tool) button to update the Cone

Axis Vector fields.

This item will appear only when the Porous Zone and Conical options are enabled.

Update From Plane Tool

(Update From Line Tool in 2D) updates the Direction- Vector and (in 3D) the Direction- Vector

from the plane tool orientation. If the Conical option is enabled, this button will update the Cone

Axis Vector and the Point on Cone Axis. See Defining the Viscous and Inertial Resistance Coeffi-

cients (p. ) for details.This item will appear only when the Porous Zone option is enabled.

Direction- Vector, Direction- Vector

indicate the directions for which the resistance coefficients are defined. See Defining the Viscous and

Inertial Resistance Coefficients (p. ) for details.These items will appear only when the Porous Zone

option is enabled, but the Conical option is not. (In 2D, only Direction- Vector will appear.)

Cone Axis Vector

specifies the X,Y,Z vector for the cone’s axis.

Point on Cone Axis

specifies a point on the cone’s axis.This point will be used by ANSYS Fluent to transform the resistances

to the Cartesian coordinate system.

Relative Velocity Resistance Formulation

allows ANSYS Fluent to either apply the relative reference frame or the absolute reference frame.This

allows for the correct prediction of the source terms.

Viscous Resistance, Inertial Resistance

contain inputs for the viscous resistance coefficient

and the inertial resistance coefficient

in

each direction. See Defining the Viscous and Inertial Resistance Coefficients (p. ) for details.These

items will appear only when the Porous Zone option is enabled.

Alternative Formulation

provides better stability to the calculation when your porous medium is anisotropic.

If you have enabled the Conical option, Direction- is the cone axis direction, Direction- is

the normal to the cone surface (radial ( ) direction for a cylinder), and Direction- is the cir-

cumferential ( ) direction.

Power Law Model

contains inputs for the C0 and C1 coefficients in the power law model for porous media. See Using

the Power-Law Model (p. ) for details.

Fluid Porosity

contains an additional input for the porous medium. See User Inputs for Porous Media (p. ) for

details.

Porosity

sets the volume fraction of fluid within the porous region.

Heat Transfer Settings

contains heat transfer settings for the porous medium. See Specifying the Heat Transfer Settings (p. )

Thermal Model

specifies whether or not thermal equilibrium is assumed between the medium and the fluid flow.

Equilibrium

specifies that the medium and the fluid flow are in thermal equilibrium in the porous medium.

Non-Equilibrium

specifies that the medium and the fluid flow are not in thermal equilibrium in the porous

medium, so that a dual cell approach is enabled.

Solid Material Name

specifies the solid material in the porous region.This drop-down menu is only available when

Equilibrium is selected from the Thermal Model list.

Solid Zone

displays the name of the solid cell zone that is coupled with the porous fluid zone through heat

transfer.This field is only displayed when Non-Equilibrium is selected from the Thermal Model

list.

Interfacial Area Density

specifies

(as described in Non-Equilibrium Thermal Model Equations (p. )) for the porous

region.This text-entry box is only available when Non-Equilibrium is selected from the Thermal

specifies

Anisotropic Species Diffusion

allows you to model anisotropic species diffusion in porous media.When this option is selected, you

can specify the Matrix Components for the anisotropic diffusion matrix in the porous zone.This

option is available only with the species transport models.

3D Fan Zone

provides the settings that define a 3D fan zone. See 3D Fan Zones (p. ) for details.

Geometry

allows you to define the location and size of the fan.

Inlet Fan Zone

allows you to select a boundary zone of type interior that will act as the surface on which the fan

will be located.

Hub Radius

defines the radius of the fan hub, that is, the inner radius of the blade-swept volume on which

the fan’s distributed momentum sources are applied.

Tip Radius

Hub Radius

Tip Radius

defines the radius of the blade tips of the fan, that is, the outer radius of the blade-swept volume

on which the fan’s distributed momentum sources are applied.

Thickness

defines the thickness of the toroid region swept by the blades in the axial direction.

Inflection Point

is a ratio that defines the fraction of the fan blade length (starting at the hub) over which the

tangential velocity of the fan discharge is increasing with increasing radius and peaks, before

tapering off (see Figure . :The Inflection Point Ratio of a Pitched Blade Turbine (p. )).

Fan Origin

defines the X, Y, and Z coordinates of a point on the Inlet Fan Zone that is the origin for the fan.

allows you to define how the fan behaves.

Rotational Direction

allows you to define the fan’s rotational direction, using the right-hand rule with respect to the

fan direction vector (that is, a vector from the Fan Origin that points into the 3D fan zone perpen-

dicular to the Inlet Fan Zone).

Operating Angular Velocity

defines the angular velocity of the fan during the simulation.

Limit Flow Rate Through Fan

specifies that the flow rate through the fan adheres to minimum and maximum values, as defined

in the Flow Rate group box.

Flow Rate

allows you to define the Maximum and Minimum flow rates through the fan.This group box is

available when the Limit Flow Rate Through Fan option is enabled.

Tangential Source Term

enables a momentum source in the tangential direction, based on impeller theory.

Radial Source Term

enables a momentum source in the radial direction, based on impeller theory.

Axial Source Term

enables a momentum source in the axial direction, based on the settings in the Axial Source

Term Settings group box.

Axial Source Term Settings

allows you to define the momentum source in the axial direction.This group box is only available

when the Axial Source Term option is enabled.

Method

specifies whether a constant pressure or a fan curve (that is, a curve created from data points

that plot pressure rise vs. volumetric flow rate) defines the axial momentum source.

Pressure Jump

defines the pressure jump that is applied across the 3D fan.This setting is only available when

constant pressure is selected for the Method.

Read Fan Curve...

allows you to read a tab-delimited ASCII file that defines the relationship between pressure

and flow rate for each 3D fan cell zone (see 3D Fan Curve File Format (p. ) for details).This

button is only available when fan curve is selected for the Method.

Curve Fitting Method

specifies whether Fluent should apply a polynomial or piecewise-linear fitting method to

construct a curve from the data points in the fan curve file.This drop-down list is only available

when fan curve is selected for the Method.

Order of Polynomial

defines the order of the polynomial curve fitting method.This setting is only available when

polynomial is selected for the Curve Fitting Method.

Initial Flow Rate

specifies your best estimate of the initial flow rate through the fan.This setting is only available

Test Angular Velocity

specifies the angular velocity of the fan used in the experiment that generated the fan curve

data.This setting is only available when fan curve is selected for the Method.

Test Temperature

specifies the temperature of the fluid flowing through the fan during the experiment that

generated the fan curve data.This setting is only available when fan curve is selected for the

Method.

Reaction

lists the parameters for reactions in the porous zone.

Reaction Mechanism

allows you to specify a defined group, or mechanism, of available reactions. See Defining Zone-Based

Reaction Mechanisms (p. ) for details about defining reaction mechanisms.

Surface-to-Volume Ratio

specifies the surface area of the pore walls per unit volume (

), and can be thought of as a measure

of catalyst loading.With this value, ANSYS Fluent can calculate the total surface area on which the

reaction takes place in each cell by multiplying

by the volume of the cell.

defines a source of heat, mass, momentum, turbulence, species, or other scalar quantity within the fluid

zone.

allows you to specify which variables in the fluid zone are fixed (as a constant value or as defined

by a profile or user-defined function), rather than computed during the calculation. See Fixing the

Values of Variables (p. ) for details.

Local Coordinate System for Fixed Velocities

enables the specification of fixed cylindrical velocity components instead of Cartesian components.

The local coordinate system is defined by the Rotation-Axis Origin and Rotation-Axis Direction.

This item is available only in 3D, and only when the Fixed Values option is on.

allows you to set parameters that are specific to the multiphase models.

Compressive Scheme Slope Limiter

ranges from  to . For example, a Compressive Scheme Slope Limiter of  corresponds to first order

upwind behavior, a value of  corresponds to second order upwind, and a value of  applies the

compressive scheme.The Multiphase tab is available only if Zonal Discretization is enabled in the

Multiphase Model Dialog Box (p. ).

Numeric Beach Treatment

is available when Open Channel Flow and/or Open Channel Wave BC is enabled in the Multiphase

Model dialog box (see Numerical Beach Treatment for Open Channels (p. ) for more detail).

Numerical Beach

when enabled expands the dialog box where you can specify the numerical beach parameters.

Beach Group ID

represents the cell zones sharing the damping length containing the same input parameters.

Damping Type

allows you to choose between One Dimensional and Two Dimensional damping.

One Dimensional

is the damping treatment in the flow direction.

Two Dimensional

is the damping treatment in the flow and gravity direction.

Compute From Inlet Boundary

is set to none by default. If there are available open channel boundaries (velocity-inlet, pressure-

inlet, and mass-flow-inlet), boundary names are added to the drop-down list. If you select a

boundary from the list, the Level Inputs, Damping Length Inputs in Flow Direction, and

Damping Resistance values will be updated in the interface.You have the option to overwrite

the updated inputs with values that are more applicable to your simulation.

Level Inputs

is only available for the Two Dimensional damping type.

Free Surface Level

is the same definition as for open channel flow, see Modeling Open Channel Flows (p. ).

Bottom Level

is the same definition as for open channel flow, see Modeling Open Channel Flows (p. ),

and is valid only for shallow waves.The bottom level is used for calculating the liquid height.

is the X,Y, and Z (for 3D) components.

Damping Length Inputs in Flow Direction

are required to calculate the start and end points of the damping length in the flow direction.

Damping Length Specification

is only available if Open Channel Wave BC is enabled in the Multiphase Model dialog box.

There are two options you can choose from End Point and Wave Lengths or End and Start

Points.

End Point

is the end point of the damping zone.

Start Point

is the starting point in the flow direction.

is updated automatically if the boundary is selected from the Compute From Inlet Boundary

Number Of Wave Lengths

is set to  by default for the calculation of the damping length.

calculates the source term using relative velocities in the numerical beach zone when using

moving/deforming meshes or moving reference frames.

Linear Damping Resistance

is the resistance per unit time.

Quadratic Damping Resistance

is the resistance per unit length.

The Solid dialog box sets the boundary conditions for a solid cell zone. It is opened from the Cell Zone

Conditions Task Page (p. ). See Inputs for Solid Zones (p. ) for details about the items below.

Controls

Zone Name

selects the material type of the solid. Materials are defined with the Materials Task Page (p. ).

details.

enables the specification of a volumetric source of energy.When you turn on this option, the Source

Term tab will allow you to specify the value for the energy source. See Defining Mass, Momentum, Energy,

and Other Sources (p. ) for details.

enables the fixing of the value of one or more variables in the solid zone, rather than computing

them during the calculation. See Fixing the Values of Variables (p. ) for details.

Important

specifies whether or not the solid zone participates in radiation.This option appears when you are using

UDF

UDF

Source Term

lists the parameters for volumetric source of energy.

Energy

displays the total number of energy sources used.

User Scalar n

displays the total number of scalars used.

allows you to specify which variables in the solid zone are fixed (as a constant value or as defined

The Copy Conditions dialog box allows you to copy cell zone and/or boundary conditions from one

zone/boundary to other zones/boundaries of the same type. It is opened either from the Cell Zone

Conditions Task Page (p. ) or from the Boundary Conditions Task Page (p. ). See Copying Cell

Controls

From Zone

specifies the zone that has the conditions you want to copy.

To Zones

specifies the zone or zones to which you want to copy the conditions.

Phase

specifies the phase for which cell zone conditions or boundary conditions are being copied.This item

appears if the VOF, mixture, or Eulerian multiphase model is being used. See Steps for Copying Cell Zone

and Boundary Conditions (p. ) for details.

Copy

copies the cell zone conditions or boundary conditions, setting all of the conditions for the zones selected

in the To Zones list to be the same as the conditions for the zone selected in the From Zone list.

The Operating Conditions dialog box allows you to set parameters related to operating conditions

in your model.

Controls

Pressure

contains items related to the modeling of pressure.

Floating Operating Pressure

specifies the use of a floating operating pressure. See Floating Operating Pressure (p. ) for details.

This option appears only for time-dependent compressible flows.

sets the operating pressure for the problem. For all flows, ANSYS Fluent uses gauge pressure internally.

Any time an absolute pressure is needed, it is generated by adding the operating pressure to the rel-

ative pressure. See Operating Pressure (p. ) for a detailed description of operating pressure and

how to set it.

Reference Pressure Location

sets the location of the cell whose pressure value is used to adjust the gauge pressure field for incom-

pressible flows that do not involve any pressure boundaries. See Reference Pressure Location (p. )

Real Gas State

allows you to specify the operating conditions in the subcritical regime of your model. Note that if the

operating conditions in your model are entirely in the supercritical regime, this setting will have no effect.

Note

This option appears only when a Cubic Equation of State Real Gas model is chosen.

Vapor

is the default option, and therefore assumes that the real gas state is vapor.

Liquid

assumes that the real gas state is liquid.

Gravity

contains inputs for gravitational acceleration, the Boussinesq model, and variable density.

Gravity

sets the ,

only in 3D solvers.) See Natural Convection and Buoyancy-Driven Flows (p. ) for details about

buoyancy-driven flows.This option appears only when Gravity is enabled.

Boussinesq Parameters

contains inputs related to the Boussinesq model.This option appears only if Energy (in the Energy

Dialog Box (p. )) and Gravity are enabled. See The Boussinesq Model (p. ) for more information

on the Boussinesq model.

Operating Temperature

sets the operating temperature (

in Equation . (p. )) for use with the Boussinesq approx-

imation.

Variable-Density Parameters

imation.

contains inputs related to the modeling of variable density.This option appears only when Gravity

Specified Operating Density

enables the specification of operating density. See Operating Density (p. ) for details.

Operating Density

sets the operating density (

in Equation . (p. )).This parameter can be set only when

Specified Operating Density is enabled.

The Select Input Parameter dialog box allows you to choose from a listing of existing input parameters

as well as to create and define new input parameters. For more information about parameters, see

Defining and Viewing Parameters (p. ) in the User's Guide, and see Working With Input and Output

Parameters in Workbench in the ANSYS Fluent in Workbench User's Guide.

Controls

contains a list of existing compatible input parameters

Current Value

displays the value of the currently selected parameter.

Used In

lists any variables that are already associated with the currently selected parameter.

Use Constant

allows you to change the associated parameter to a constant (that is, real) value.

New Parameter

opens the Parameter Expression Dialog Box (p. ), in which you can assign names and values to an input

parameter.

The Profiles dialog box allows you to define new profiles by reading cell zone and boundary profile

files. You can also examine the existing profile definitions and delete unused profiles. See Profiles (p. )

for details about cell zone and boundary profiles.

Controls

Profile

contains a selectable list of available profiles.When a profile is selected its available fields are displayed

under Fields.

Fields

displays the fields available in the selected profile. After the profile file has been read, these fields will

also appear in any boundary condition dialog box (for example, the Velocity Inlet dialog box) that allows

profile specification of a variable.To the right of (or below) the variable in the boundary conditions dialog

box, there will be a drop-down list that contains a constant and the fields from available profile files.To

use a particular profile field, just select it from the list.

Interpolation Method

allows you to select the interpolation method for the profile selected from the Profile list.This selection

is only available for point profiles, and will only take effect when the Apply button is clicked.The choices

include the following:

Constant

specifies that ANSYS Fluent should use zeroth-order interpolation to assign the point profile values

to the nearest cell faces at the boundary.This is the default selection.

specifies that ANSYS Fluent should assign a value to each cell face at the boundary based on weighted

contributions from the values in the point profile file.The weighting factor is inversely proportional

to the distance between the profile point and the cell face center.

specifies that ANSYS Fluent should assign values to the cell faces at the boundary through a first-order

interpolation method that tries to minimizes the sum of the squares of the offsets (residuals) between

the profile data points and the cell face centers.

allows you to attach the profile to a reference frame. If you select a reference frame other than global,

then the profile will follow the orientation and/or motion of the specified reference frame.

Delete

deletes the selected profile from memory.

Replicate...

opens the Replicate Profile Dialog Box (p. ), in which you can reorient and scale the profile.This item

appears only in 3D.

Orient...

opens the Orient Profile Dialog Box (p. ), in which you can reorient and scale the profile.This item appears

only in 3D.

Read...

opens The Select File Dialog Box (p. ) so that you can read a boundary profile file. If a profile in the file

has the same name as an existing profile, the old profile will be overwritten.

Write...

opens the Write Profile Dialog Box (p. ), in which you can save profile data.

Apply

sets the selection made in the Interpolation Method list for point profiles in preparation for interpolation.

The profile is not actually interpolated until a profile field is selected in a boundary condition dialog box

(for example, the Velocity Inlet dialog box) and the solution is initialized.

The Replicate Profile dialog box allows you to replicate a profile periodically, typically for use as a

boundary condition in a turbomachinary case. See Replicating Profiles (p. ) for details.

Controls

Controls

Current profile

shows the name of the currently selected profile in the Profiles Dialog Box (p. ).This is the profile on

which the new profile will be based.

New Profile

sets the name of the new cell zone or boundary profile.

New Field Definitions

contains inputs and controls for the definition of the vector and scalar fields in the new profile.

New Fields

sets the number of data fields in the new profile.

New Field Names

contains inputs for the names of the data fields in the new profile. For a vector field, all  inputs in

each row will be active; for a scalar field, only the first will be active.

Compute From...

contains drop-down lists with the names of the fields in the Current profile. In these lists, select the

fields from which the New Field Names will be computed.

Treat as Scalar Quantity

indicates (if on) that the adjacent field is a scalar quantity. If this option is off, the field is a vector

quantity.

Current Profile Definitions

contains inputs for the replication of the new profile.

Full  deg.

automatically determines the number of copies of the original profile that are needed to make the

full  degree profile based on the other information you specify

Number of copies

specifies how many copies of the original profile are created.

Number of sectors in  deg.

the number of periodic sections, based on the original profile, that are present in  degrees.

Number of sectors in profile

the number of periodic sections in the original profile.

Calculated angle

(for display only) the angle occupied by the original profile.

Create

creates a new profile using the information specified in the dialog box.

Create

The Orient Profile dialog box allows you to reorient a profile so that you can apply it to a particular

boundary. See Reorienting Profiles (p. ) for details.

Controls

New Fields

quantity.

Orient To...

contains inputs for the definition of the local coordinate system for the new profile.This coordinate system

will determine the orientation of the profile.

Direction Vector

is the vector that translates a cell zone or boundary profile to the new position, and is defined between

the centers of the profile fields.

Rotation Matrix [RM

] specifies the rotational matrix

, which is based on Euler angles ( ,

, and ) that define an ortho-

gonal system

as the result of the three successive rotations from the original system

. See

Reorienting Profiles (p. ) for more information.

Create

The Write Profile dialog box allows you to create a profile file from the conditions on a specified cell

zone or boundary/surface. See Writing Profile Files (p. ) for details on writing profile files.

Controls

Options

contains options for writing profiles.

Define New Profiles

enables the creation of a profile file from the conditions on a specified boundary or surface.

Write Currently Defined Profiles

enables the creation of a profile file containing all profiles that are currently defined.

Merge Profile Options

Write Merge Profiles

(only available if two or more surfaces are selected) writes a .csv file with the selected surfaces

consolidated into one set of data points.

Surfaces

contains a list from which you can select the surface(s) from which you want to extract data.

Values

contains a list from which you can select the variable(s) for which you want to create profiles.

Write...

opens The Select File Dialog Box (p. ), in which you can specify a filename for the profile file.

The Boundary Conditions task page allows you to set the type of a boundary and display other dialog

boxes to set the boundary condition parameters for each boundary.

Boundary Conditions Task Page

Controls

Zone

Controls

Zone

contains a selectable list of boundary zones from which you can select the zone of interest.You can check

a zone type by using the mouse probe (see Controlling the Mouse Button Functions (p. )) on the displayed

physical mesh.This feature is particularly handy if you are setting up a problem for the first time, or if you

have two or more boundary zones of the same type and you want to determine the zone IDs.To do this

you must first display the mesh with the Mesh Display Dialog Box (p. ).Then click the boundary zone

with the right (select) mouse button. ANSYS Fluent will print the zone ID and type of that boundary zone

in the console window.

Phase

specifies the phase for which conditions at the selected boundary Zone are being set.This item appears

if the VOF, mixture, or Eulerian multiphase model is being used. See Defining Multiphase Cell Zone and

Type

contains a drop-down list of boundary condition types for the selected zone.The list contains all possible

types to which the zone can be changed.

Important

Note that you cannot use this method to change zone types to or from the periodic type,

since additional restrictions exist for this boundary type. Creating Periodic Zones and

Interfaces (p. ) explains how to create and uncouple periodic zones.

ID

displays the zone ID number of the selected zone. (This is for informational purposes only; you cannot edit

this number.)

Edit...

opens the appropriate dialog box for setting the boundary conditions for that particular boundary type.

Copy...

Edit...

Copy...

opens the Copy Conditions Dialog Box (p. ), which allows you to copy boundary conditions from one

zone to other zones of the same type. See Copying Cell Zone and Boundary Conditions (p. ) for details.

Periodic Conditions...

opens the Periodic Conditions Dialog Box (p. ).

Highlight Zone

when enabled highlights the boundary zone (selected in the task page) in the graphics window.

... Axis Dialog Box

... Degassing Dialog Box

... Exhaust Fan Dialog Box

... Fan Dialog Box

... Inlet Vent Dialog Box

... Intake Fan Dialog Box

... Interface Dialog Box

... Interior Dialog Box

... Mass-Flow Inlet Dialog Box

... Mass-Flow Outlet Dialog Box

... Outflow Dialog Box

... Outlet Vent Dialog Box

... Periodic Dialog Box

... Porous Jump Dialog Box

... Pressure Far-Field Dialog Box

... Pressure Inlet Dialog Box

... Pressure Outlet Dialog Box

... Radiator Dialog Box

... RANS/LES Interface Dialog Box

... Symmetry Dialog Box

...Velocity Inlet Dialog Box

...Wall Dialog Box

... Periodic Conditions Dialog Box

The Axis dialog box can be used to modify the name of an axis zone; there are no conditions to be

set. It is opened from the Boundary Conditions Task Page (p. ). See Axis Boundary Conditions (p. )

for information about axis boundaries.

Controls

Zone Name

Controls

Zone Name

Phase

displays the name of the phase.This item appears if the VOF, mixture, or Eulerian multiphase model is

The Degassing dialog box can be used to modify the name of a degassing zone; there are no conditions

to be set. It is opened from the Boundary Conditions Task Page (p. ). See Degassing Boundary

Conditions (p. ) for information about axis boundaries.

Controls

Zone Name

Phase

displays the name of the phase.

The Exhaust Fan dialog box sets the boundary conditions for an exhaust fan zone. It is opened from

the Boundary Conditions Task Page (p. ). See Inputs at Exhaust Fan Boundaries (p. ) for details

about defining the items below.

Controls

Zone Name

Phase

displays the name of the phase. It appears only for multiphase flows.

Momentum

contains the momentum parameters.

Backflow Reference Frame

specify whether backflow temperature, pressure, and flow directions are in the Absolute or Relative

to the Adjacent Cell Zone reference frame.

sets the gauge pressure at the outlet boundary.

Backflow Direction Specification Method

sets the direction of the inflow stream should the flow reverse direction.You can choose Direction

Vector, Normal to Boundary,or From Neighboring Cell.

Coordinate System

contains a drop-down list for selecting the coordinate system.You can choose Cartesian, Cylindrical,

or Local Cylindrical.This option is available only when Direction Vector is selected from the Backflow

Direction Specification Method drop-down list.

X-,Y-, Z-Component of Flow Direction

allows you to specify the velocity components in x, y, and z directions respectively.This option is

available when Cartesian is selected for the Coordinate System.

Radial-,Tangential-, Axial-Component of Flow Direction

set the direction of the flow at the boundary.These items will appear for 2D axisymmetric cases, or

for 3D cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.

Backflow Pressure Specification

specifies how the pressure is calculated under backflow conditions. If you select Static Pressure, the

Gauge Pressure is directly imposed as the boundary face pressure; if you select Total Pressure, the

Gauge Pressure will be combined with a dynamic contribution that is based on the velocity in the

adjacent cell zone.

specifies the rise in pressure across the fan. See Specifying the Pressure Jump (p. ) for details.

sets the X, Y, and Z coordinates of the origin of the local cylindrical coordinate system.

sets the X, Y, and Z components of the direction of the local cylindrical coordinate system.

Turbulence

displays the turbulence parameters.

Specification Method

specifies which method will be used to define the turbulence parameters.You can choose K and

Epsilon ( -  models and RSM only), K and Omega ( -

models only), Intensity and Length

Scale, Intensity and Viscosity Ratio, Intensity and Hydraulic Diameter, Modified Turbulent

Viscosity (Spalart-Allmaras model only), or Turbulent Viscosity Ratio (Spalart-Allmaras model

only). See Determining Turbulence Parameters (p. ) for information about the inputs for each

of these methods. (This item will appear only for turbulent flow calculations.)

Backflow Turbulent Kinetic Energy, Backflow Turbulent Dissipation Rate

set values for the turbulence kinetic energy  and its dissipation rate .These items will appear

if you choose K and Epsilon as the Specification Method.

Backflow Turbulent Kinetic Energy, Backflow Specification Dissipation Rate

set values for the turbulence kinetic energy  and its specific dissipation rate

.These items will

appear if you choose K and Omega as the Specification Method.

Backflow Turbulent Intensity, Backflow Turbulent Length Scale

set values for turbulence intensity  and turbulence length scale .These items will appear if you

choose Intensity and Length Scale as the Specification Method.

Backflow Turbulent Intensity, Backflow Turbulent Viscosity Ratio

set values for turbulence intensity  and turbulent viscosity ratio

.These items will appear

if you choose Intensity and Viscosity Ratio as the Specification Method.

Backflow Turbulent Intensity, Backflow Hydraulic Diameter

set values for turbulence intensity  and hydraulic diameter .These items will appear if you

choose Intensity and Hydraulic Diameter as the Specification Method.

Backflow Modified Turbulent Viscosity

sets the value of the backflow modified turbulent viscosity .This item will appear if you choose

Modified Turbulent Viscosity as the Specification Method.

sets the value of the backflow turbulent viscosity ratio

.This item will appear if you choose

Turbulent Viscosity Ratio as the Specification Method.

Reynolds-Stress Specification Method

specifies which method will be used to determine the backflow Reynolds stress boundary condi-

tions when the Reynolds stress turbulence model is used.You can choose either K or Turbulence

Intensity or Reynolds-Stress Components. If you choose the former, ANSYS Fluent will compute

the Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds

stresses yourself. See Reynolds Stress Model (p. ) for details. (This item will appear only for RSM

turbulent flow calculations.)

Backflow UU,VV,WW, UV,VW, UW Reynolds Stresses

specify the backflow Reynolds stress components when Reynolds-Stress Components is chosen

as the Reynolds-Stress Specification Method.

Thermal

contains the thermal parameters.This parameter is available only when the energy equation is turned

on.

sets the total temperature of the inflow stream should the flow reverse direction.

Radiation

contains the boundary conditions for the radiation model at the exhaust fan.

External Black Body Temperature Method, Internal Emissivity

set the radiation boundary conditions when you are using the P-, DTRM, DO, S2S, or MC models for

radiation heat transfer. See Defining Boundary Conditions for Radiation (p. ) for details.

Participates in Solar Ray Tracing

specifies whether or not the fan participates in solar ray tracing.

Solar Transmissivity Factor

specifies a multiplier (ranging from  to ) that is applied to the solar irradiation entering the domain

through the fan.

Participates in View Factor Calculation

specifies whether or not the fan participates in the view factor calculation as part of the S2S radiation

model.This parameter is available only if you select the Surface to Surface radiation model.

Species

contains the species parameters.

Specify Species in Mole Fractions

allows you to specify the species in mole fractions rather than mass fractions.

Mean Mixture Fraction, Mixture Fraction Variance

set inlet values for the PDF mixture fraction and its variance. (These items will appear only if you are

using the non-premixed or partially premixed combustion model.)

Secondary Mean Mixture Fraction, Secondary Mixture Fraction Variance

set inlet values for the secondary mixture fraction and its variance. (These items will appear only if

you are using the non-premixed or partially premixed combustion model with two mixture fractions.)

Species Mass Fractions

contains inputs for the mass fractions of defined species. See Defining Cell Zone and Boundary Con-

ditions for Species (p. ) for details about these inputs.These items will appear only if you are

modeling non-reacting multi-species flow or you are using the finite-rate reaction formulation.

Backflow Progress Variable

sets the value of the progress variable for premixed turbulent combustion. See Setting Boundary

Conditions for the Progress Variable (p. ) for details.

This item will appear only if the premixed or partially premixed combustion model is used.

DPM

contains the discrete phase parameters.This tab is available only if you have defined at least one injection.

Discrete Phase BC Type

sets the way that the discrete phase behaves with respect to the boundary.This item appears when

one or more injections have been defined.

reflect

rebounds the particle off the boundary with a change in its momentum as defined by the coefficient

of restitution (see Particle Reflection at Wall in the Fluent Theory Guide).

trap

terminates the trajectory calculations and records the fate of the particle as “trapped”. In the case

of evaporating droplets, their entire mass instantaneously passes into the vapor phase and enters

escape

reports the particle as having “escaped” when it encounters the boundary.Trajectory calculations

are terminated. See Figure . :“Escape” Boundary Condition for the Discrete Phase (p. ).

wall-jet

indicates that the direction and velocity of the droplet particles are given by the resulting mo-

mentum flux, which is a function of the impingement angle. See Figure . :“Wall Jet” Boundary

Condition for the Discrete Phase in the Theory Guide.

specifies a user-defined function to define the discrete phase boundary condition type.

Discrete Phase BC Function

sets the user-defined function from the drop-down list.

contains the multiphase parameters.

Backflow Granular Temperature

motion of the particles.

Volume Fraction Specification Method

sets the method used to specify the volume fraction of the secondary phase selected in the Boundary

Conditions Task Page (p. ).This section of the dialog box will appear when one of the multiphase

models is being used. See Defining Multiphase Cell Zone and Boundary Conditions (p. ) for details.

Backflow Volume Fraction

specifies the volume fraction of the secondary phase as a constant, profile, of UDF function.

From Neighboring Cell

calculates the volume fraction from the neighboring cells.

Potential

displays the boundary conditions for the electric potential field.This tab is available only if you have enabled

either the Electric Potential model or the Electrochemical reaction model in the Species Dialog

Box (p. ).

Potential Boundary Condition

is a drop-down list of available potential boundary condition types: Specified Flux and Specified

Value. For the Specified Flux boundary condition, you will need to specify Current Density at the

wall. For the Specified Value boundary condition, you will need to specify Potential at the wall.

UDS

contains the UDS parameters.

User-Defined Scalar Boundary Condition

appears only if user-defined scalars are specified.

specifies whether the scalar is a specified flux or a specified value.

User-Defined Scalar Boundary Value

specifies the value of the scalar.

The Fan dialog box sets the boundary conditions for a fan zone. It is opened from the Boundary

Conditions Task Page (p. ). See User Inputs for Fans (p. ) for details about the items below.

Controls

Zone Name

Pressure-Jump Specification

contains inputs that define the pressure jump across the fan.

Reverse Fan Direction

sets the fan flow direction relative to the zone direction. If Zone Average Direction is pointing in the

direction you want the fan to blow, do not select Reverse Flow; if it is pointing in the opposite direction,

select Reverse Flow.

Zone Average Direction

displays the (face-averaged) direction vector for the zone as an aid in determining whether or not

you want to select Reverse Flow.

Profile Specification of Pressure-Jump

enables the use of a boundary profile or user-defined function for the pressure jump specification.

See Profiles (p. ) or the Fluent Customization Manual for details.When this option is enabled,

Pressure Jump Profile will appear in the dialog box and the next four items below it will not.

Pressure Jump Profile

contains a drop-down list from which you can select a boundary profile or a user-defined function

for the pressure jump definition.This item will appear if you enable Profile Specification of Pressure-

Jump.

Pressure-Jump

specifies the pressure-jump as a constant value or as a polynomial, piecewise-linear, or piecewise-

polynomial function of velocity. See Defining the Pressure Jump (p. ) for details.

Limit Polynomial Velocity Range

limits the minimum and maximum velocity magnitudes used to calculate the pressure jump when it

is defined as a function of velocity.

Min Velocity Magnitude, Max Velocity Magnitude

specify the minimum and maximum values to which the velocity magnitude is limited (when the

Limit Polynomial Velocity Range option is enabled).

Calculate Pressure-Jump from Average Conditions

enables the option to use the mass-averaged velocity normal to the fan to determine a single pressure-

interior

allows the particles to pass through the boundary.

reflect

of restitution. (See Particle Reflection at Wall in the Fluent Theory Guide.)

trap

escape

wall-jet

Swirl-Velocity Specification

contains inputs for the specification of fan swirl velocity.This section of the dialog box appears only for

3D models.

enables the specification of a swirl velocity for the fan.

Fan Axis

sets the direction vector for the fan’s axis of rotation.

Fan Origin

sets the origin in the global coordinate system through which the fan rotation axis passes.

Fan Hub Radius

set the radius of the hub.The default is 1e- to avoid division by zero in the polynomial.

Profile Specification of Tangential Velocity

enables the use of a boundary profile or user-defined function for the tangential velocity specification.

Tangential Velocity Profile will appear in the dialog box and Tangential-Velocity Polynomial

Coefficients will not.

Tangential Velocity Profile

for the definition of the tangential velocity.This item will appear if you enable Profile Specification

of Tangential Velocity.

Tangential-Velocity Polynomial Coefficients

sets the coefficients for the tangential velocity polynomial. Separate the coefficients by spaces.

Profile Specification of Radial Velocity

enables the use of a boundary profile or user-defined function for the radial velocity specification.

See Profiles (p. ) or the Fluent Customization Manual for details.When this option is enabled, Ra-

dial Velocity Profile will appear in the dialog box and Radial-Velocity Polynomial Coefficients will

not.

Radial Velocity Profile

for the definition of the radial velocity.This item will appear if you enable Profile Specification of

Radial Velocity.

Radial-Velocity Polynomial Coefficients

sets the coefficients for the radial velocity polynomial. Separate the coefficients by spaces.

The Inlet Vent dialog box sets the boundary conditions for an inlet vent zone. It is opened from the

Boundary Conditions Task Page (p. ). See Inputs at Inlet Vent Boundaries (p. ) for details about

defining the items below.

Controls

Zone Name

Momentum

specifies the reference frame for the inlet vent. If the cell zone adjacent to the inlet vent is moving,

you can choose to specify relative or absolute velocities by selecting Relative to Adjacent Cell Zone

or Absolute in the Reference Frame drop-down list.

sets the gauge total (or stagnation) pressure of the inflow stream. If you are using moving reference

frames, see Defining Total Pressure and Temperature (p. ) for information about relative and absolute

total pressure.

sets the static pressure on the boundary when the flow becomes (locally) supersonic. It is also used

to compute initial values for pressure, temperature, and velocity if the inlet vent boundary condition

is selected for computing initial values (see Initializing the Entire Flow Field Using Standard Initializa-

specifies the method you will use to define the flow direction. If you choose Direction Vector, you

will define the flow direction components, and if you choose Normal to Boundary no inputs are re-

quired. See Defining the Flow Direction (p. ) for information on specifying flow direction.

specifies whether Cartesian, Cylindrical, Local Cylindrical, Local Cylindrical Swirl vector components

will be specified.This item will appear only for 3D cases in which you have selected Direction Vector

as the Direction Specification Method.

X,Y,Z-Component of Flow Direction

set the direction of the flow at the inlet boundary.These items will appear if the selected Coordinate

System is Cartesian or the model is 2D non-axisymmetric.

Radial,Tangential, Axial Component of Flow Direction

set the direction of the flow at the inlet boundary.These items will appear for 2D axisymmetric cases,

or for 3D cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.

Loss-Coefficient

sets the non-dimensional loss coefficient used to compute the pressure drop. See Specifying the Loss

Coefficient (p. ) for details.

lists the turbulence parameters.

Turbulent Kinetic Energy,Turbulent Dissipation Rate

Turbulent Kinetic Energy, Specific Dissipation Rate

Turbulence Intensity,Turbulence Length Scale

Turbulence Intensity,Turbulent Viscosity Ratio

Turbulence Intensity, Hydraulic Diameter

sets the value of the modified turbulent viscosity .This item will appear if you choose Modified

Turbulent Viscosity as the Specification Method.

sets the value of the turbulent viscosity ratio

.This item will appear if you choose Turbulent

Viscosity Ratio as the Specification Method.

specifies which method will be used to determine the Reynolds stress boundary conditions when

the Reynolds stress turbulence model is used.You can choose either K or Turbulence Intensity

or Reynolds-Stress Components. If you choose the former, ANSYS Fluent will compute the

Reynolds stresses for you. If you choose the latter, you will explicitly specify the Reynolds stresses

yourself. See Reynolds Stress Model (p. ) for details. (This item will appear only for RSM turbulent

flow calculations.)

UU,VV,WW, UV,VW, UW Reynolds Stresses

specify the Reynolds stress components when Reynolds-Stress Components is chosen as the

Reynolds-Stress Specification Method.

Thermal

contains the thermal parameters.

sets the total temperature of the inflow stream. If you are using moving reference frames, see Defining

Total Pressure and Temperature (p. ) for information about relative and absolute total temperature.

Radiation

contains the radiation parameters.

Radiation

specifies whether or not the inlet vent participates in solar ray tracing.

through the inlet vent.

specifies whether or not the inlet vent participates in the view factor calculation as part of the S2S

radiation model.This parameter is available only if you select the Surface to Surface radiation model.

Species

ditions for Species (p. ) for details about these inputs. (These items will appear only if you are

modeling non-reacting multi-species flow or you are using the finite-rate reaction formulation.)

DPM

contains the discrete phase parameters.

reflect

trap

escape

wall-jet

specifies the volume fraction of the secondary phase selected in the Boundary Conditions Task

Page (p. ).This section of the dialog box will appear when one of the multiphase models is being

used. See Defining Multiphase Cell Zone and Boundary Conditions (p. ) for details.

Open Channel

is available when the VOF model with open channel flow is enabled.

Secondary Phase for Inlet

is where the specified parameters are valid only for one secondary phase. In case of a three-phase

flow, select the corresponding secondary phase from this list.This appears when Open Channel is

enabled.

Flow Specification Method

allows you to select the type of flow.You can choose Free Surface Level and Velocity, Total Height

and Velocity, or Free Surface Level and Total Height.This appears when Open Channel is enabled.

can be determined using the absolute value of height from the free surface to the origin in the direction

of gravity, or by applying the correct sign based on whether the free surface level is above or below

the origin.

Total Height

is used as an option for describing the flow. It is given by Equation . (p. ).

is valid only for shallow waves.The bottom level is used for calculating the liquid height.

sets the magnitude of the velocity vector at the inflow boundary.

Level-Set Function Flux

appears if the Level Set option is enabled for the VOF model.

Potential

Box (p. ).

UDS

The Intake Fan dialog box sets the boundary conditions for an intake fan zone. It is opened from the

Boundary Conditions Task Page (p. ). See Inputs at Intake Fan Boundaries (p. ) for details about

Controls

Zone Name

Momentum

Controls

Zone Name

Momentum

specifies the reference frame for the intake fan. If the cell zone adjacent to the intake fan is moving,

to compute initial values for pressure, temperature, and velocity if the intake fan boundary condition

specifies whether Cartesian, Cylindrical, Local Cylindrical,or Local Cylindrical Swirl vector com-

ponents will be defined.This item will appear only for 3D cases in which you have selected Direction

Vector as the Direction Specification Method.

set the direction of the flow at the inlet boundary. For compressible flow, if the inflow becomes su-

personic, the velocity is not reoriented.These items will appear if the selected Coordinate System

is Cartesian or the model is 2D non-axisymmetric.

personic, the velocity is not reoriented.These items will appear for 2D axisymmetric cases, or for 3D

cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.

consists of the turbulence parameters.

Turbulent Intensity,Turbulent Length Scale

Turbulent Intensity,Turbulent Viscosity Ratio

Turbulent Intensity, Hydraulic Diameter

the Reynolds stress turbulence model is used.You can choose either K or Turbulent Intensity

Thermal

Radiation

specifies whether or not the intake fan participates in solar ray tracing.

through the intake fan.

specifies whether or not the intake fan participates in the view factor calculation as part of the S2S

Species

Species

DPM

reflect

trap

reflect

trap

escape

wall-jet

Potential

Potential

Box (p. ).

UDS

The Interface dialog box can be used to modify the name of an interface zone; there are no conditions

to be set. It is opened from the Boundary Conditions Task Page (p. ). Interface zones are used for

multiple reference frame and sliding mesh calculations, and for non-conformal meshes. See The Multiple

Reference Frame Model (p. ), Setting Up the Sliding Mesh Problem (p. ), and Non-Conformal

Meshes (p. ) for details.

Controls

Zone Name

Non-Overlapping Zone

displays the name of the non-overlapping zone created for this interface zone as part of the creation of

a mesh interface.

Edit...

opens the boundary condition dialog box of the non-overlapping zone, so that you can easily review

and/or revise the settings.

Phase

Edit...

Phase

displays the name of the phase.This item appears only for multiphase flows.

The Interior dialog box can be used to modify the name of an interior zone; there are no conditions

to be set. It is opened from the Boundary Conditions Task Page (p. ).

Controls

Zone Name

Phase

The Mass-Flow Inlet dialog box sets the boundary conditions for a mass-flow inlet zone. It is opened

from the Boundary Conditions Task Page (p. ). See Inputs at Mass-Flow Inlet Boundaries (p. ) for

details about defining the items below.

Controls

Zone Name

Momentum

displays the momentum boundary conditions.

specifies the reference frame for the mass flow. If the cell zone adjacent to the mass-flow inlet is

moving, you can choose to specify relative or absolute velocities by selecting Relative to Adjacent

Cell Zone or Absolute in the Reference Frame drop-down list.

Mass Flow Specification Method

specifies whether you are defining Mass Flow Rate, Mass Flux, or Mass Flux with Average Mass

Flux.

sets the prescribed mass flow rate for the zone.This flow rate is converted internally to a prescribed

uniform mass flux over the zone by dividing the flow rate by the flow direction area projection of the

zone.This item will appear if you selected Mass Flow Rate in the Mass Flow Specification Method

list.

Important

list.

Important

Note that for axisymmetric problems, this mass flow rate is the flow rate through

the entire (

Mass Flux

sets the prescribed mass flux for the zone.This item will appear if you selected Mass Flux or Mass

Flux with Average Mass Flux in the Mass Flow Specification Method list.

Important

Note that for axisymmetric problems, this mass flux is the flux through a -radian

slice of the domain.

Average Mass Flux

sets the average mass flux through the zone. See More About Mass Flux and Average Mass Flux (p. )

for details.This item will appear if you selected Mass Flux with Average Mass Flux in the Mass Flow

Specification Method list.

Important

Supersonic/Initialization Gauge Pressure

sets the static pressure that will be used to initialize the flow field if the mass-flow inlet boundary

condition is selected for initializing flow properties (see Initializing the Entire Flow Field Using

Standard Initialization (p. )).

set the velocity-direction vector of the inflow stream.This vector does not need to be normalized (for

example, you can specify the vector (  ) rather than (. . . )).These items will appear

if the selected Coordinate System is Cartesian or the model is 2D non-axisymmetric.

set the velocity-direction vector of the inflow stream.These items will appear for 2D axisymmetric

cases, or for 3D cases for which the selected Coordinate System is Cylindrical or Local Cylindrical.

Axial-, Radial-Component of Flow Direction,Tangential-Velocity

appear for a 3D Local Cylindrical Swirl coordinate system.

sets the X, Y, and Z coordinates of the origin of the local cylindrical (swirl) coordinate system.

sets the X, Y, and Z components of the direction of the local cylindrical (swirl) coordinate system.

contains the turbulence parameters.

Acoustic Wave Model

contains settings for treatment of acoustic pressure waves at the boundary.

Off

disables special treatment of acoustic pressure waves at the boundary.

Non Reflecting

enables the general non-reflecting boundary condition treatment described in General Non-Re-

flecting Boundary Conditions (p. ).

Impedance

enables the impedance boundary condition treatment described in Impedance Boundary Condi-

Transparent Flow Forcing

enables the transparent flow forcing boundary condition described in Transparent Flow Forcing

Impedance Parameters

contains the parameters for the impedance boundary condition treatment. For details refer to Using

the Impedance Boundary Condition (p. ).

Transparent Flow Forcing Parameters

contains the parameters for the transparent flow forcing boundary condition treatment. For details

refer to Using the Transparent Flow Forcing Boundary Condition (p. ).

Thermal

sets the total temperature of the inflow stream.

Radiation

Radiation

specifies whether or not the mass-flow inlet participates in solar ray tracing.

through the mass-flow inlet.

specifies whether or not the mass-flow inlet participates in the view factor calculation as part of the

S2S radiation model.This parameter is available only if you select the Surface to Surface radiation

model.

Species

Scalar Mass Fractions

(partially-premixed combustion FGM model only) allows you to specify the scalar species mass fractions

for the transported scalars that you selected in the Select Transported Scalars dialog box.

DPM

reflect

trap

escape

wall-jet

Potential

Box (p. ).

UDS

The Mass-Flow Outlet dialog box sets the boundary conditions for a mass-flow outlet zone. It is

opened from the Boundary Conditions Task Page (p. ). See Inputs at Mass-Flow Outlet Boundar-

ies (p. ) for details about defining the items below.

Controls

Controls

Zone Name

Momentum

specifies the reference frame for the mass flow when the cell zone adjacent to the mass-flow outlet

is moving.The only available option is Relative to Adjacent Cell Zone, so you must define the mass

flow relative to the adjacent cell zone.

specifies whether you are defining a Mass Flow Rate, Mass Flux, Mass Flux with Average

Mass Flux, or (if the density of the material is defined either as an ideal gas or using a real gas

model) Exit Corrected Mass Flow Rate.

zone.This item will appear if you selected Mass Flow Rate from the Mass Flow Specification

Important

Mass Flux

Flux with Average Mass Flux from the Mass Flow Specification Method drop-down list.

Important

sets the average mass flux through the zone. For details, see Defining the Mass Flow Rate or Mass

Flux (p. ).This item will appear if you selected Mass Flux with Average Mass Flux from the Mass

Flow Specification Method drop-down list.

Important

Exit Corrected Mass Flow Rate

sets the value for an exit corrected mass flow rate that is maintained by adjusting the mass flow rate

to the total conditions at the outlet.The resulting mass flow rate will be proportional to the exit total

pressure and inversely proportional to the square root of the exit total temperature (or equivalently,

inversely proportional to the stagnation speed of sound). For details, see Exit Corrected Mass Flow

Rate (p. ).This item will appear if you selected Exit Corrected Mass Flow Rate from the Mass Flow

Important

ECMF Reference Temperature

sets the reference temperature for the exit corrected mass flow rate; for details, see Exit Corrected

Mass Flow Rate (p. ).Typically, it is set to be the same as the inflow total temperature.This item

will appear if you selected Exit Corrected Mass Flow Rate from the Mass Flow Specification

ECMF Reference Gauge Pressure

sets the reference gauge pressure for the exit corrected mass flow rate; for details, see Exit Corrected

Mass Flow Rate (p. ).Typically, it is set to be the same as the inflow total pressure.This item will

appear if you selected Exit Corrected Mass Flow Rate from the Mass Flow Specification Method

set the velocity-direction vector of the outflow stream.This vector does not need to be normalized

(for example, you can specify the vector (  ) rather than (. . . )).These items will appear

set the velocity-direction vector of the outflow stream.These items will appear for 2D axisymmetric

Radiation

External Black Body Temperature Method, Black Body Temperature, Internal Emissivity

specifies whether or not the mass-flow outlet participates in solar ray tracing.

through the mass-flow outlet.

specifies whether or not the mass-flow outlet participates in the view factor calculation as part of the

model.

DPM

reflect

trap

escape

wall-jet

UDS

The Outflow dialog box sets the boundary conditions for an outflow zone. It is opened from the

Boundary Conditions Task Page (p. ). See Using Outflow Boundaries (p. ) for details about using

outflow boundaries.

Controls

Zone Name

specifies the portion of the outflow that is going through the boundary. See Mass Flow Split Boundary

set the radiation boundary conditions when you are using the P-, DTRM, DO, S2S, or MC models for ra-

diation heat transfer. See Defining Boundary Conditions for Radiation (p. ) for details.

sets the way that the discrete phase behaves with respect to the boundary.This item appears when one

or more injections have been defined.

reflect

reflect

trap

terminates the trajectory calculations and records the fate of the particle as “trapped”. In the case of

evaporating droplets, their entire mass instantaneously passes into the vapor phase and enters the

cell adjacent to the boundary. See Figure . :“Trap” Boundary Condition for the Discrete

escape

reports the particle as having “escaped” when it encounters the boundary.Trajectory calculations are

terminated. See Figure . :“Escape” Boundary Condition for the Discrete Phase (p. ).

wall-jet

indicates that the direction and velocity of the droplet particles are given by the resulting momentum

flux, which is a function of the impingement angle. See Figure . :“Wall Jet” Boundary Condition

for the Discrete Phase in the Theory Guide.

specifies whether or not outflow participate in solar ray tracing.

through the outflow.

specifies whether or not the outflow participates in the view factor calculation as part of the S2S radiation

The Outlet Vent dialog box sets the boundary conditions for an outlet vent zone. It is opened from

the Boundary Conditions Task Page (p. ). See Inputs at Outlet Vent Boundaries (p. ) for details

Controls

Zone Name

Momentum

will define the flow direction components, and if you choose Normal to Boundary or From Neigh-

boring Cell no inputs are required. See Defining the Flow Direction (p. ) for information on specifying

flow direction.

Backflow Turbulent Kinetic Energy, Backflow Specific Dissipation Rate

tions when the Reynolds stress turbulence model is used.You can choose either K or Turbulent

Thermal

sets the total temperature of the inflow stream should the flow reverse direction

Radiation

contains the boundary conditions for the radiation model at the outlet vent.

specifies whether or not the outlet vent participates in solar ray tracing.

through the outlet vent.

specifies whether or not the outlet vent participates in the view factor calculation as part of the S2S

Species

Species

DPM

reflect

trap

reflect

trap

escape

wall-jet

Potential

Box (p. ).

UDS

The Periodic dialog box sets the boundary conditions for a periodic zone. It is opened from the

Boundary Conditions Task Page (p. ). See Inputs for Periodic Boundaries (p. ) for details about

the items below. See Periodic Flows (p. ) for information about fully-developed periodic flow.

Controls

Zone Name

Periodic Type

indicates whether the periodicity of the domain is Translational or Rotational.

Periodic Pressure Jump

Controls

Zone Name

sets the pressure increase/decrease across the periodic boundary. (This item will not appear if the pressure-

based (default) solver is used; it is relevant only for the density-based solvers.)

The Porous Jump dialog box sets the boundary conditions for a porous-jump zone. It is opened from

the Boundary Conditions Task Page (p. ). See Porous Jump Boundary Conditions (p. ) for details

Controls

Zone Name

Face Permeability

sets the face permeability coefficient (  in Equation . (p. )).

Porous Medium Thickness

sets the thickness of the porous medium (

).

Pressure-Jump Coefficient

sets the pressure-jump coefficient (

).

Thermal Contact Resistance

sets the thermal contact resistance.

sets the adhesion method and contact angle.

Constrained-Two-Sided Adhesion

constrains the contact angle at the porous jump,When this option is disabled then the forced two-

sided adhesion treatment is in effect. See Jump Adhesion for more information.

Contact Angle

is the contact angle at the porous jump.

interior

reflect

trap

reflect

trap

escape

wall-jet

Solar Boundary Conditions

contains the settings for solar ray tracing.This group box is available only if you select Solar Ray Tracing

from the Model list in the Solar Load group box of the Radiation Model dialog box. See Solar Ray Tra-

cing (p. ) for details.

specifies whether or not the porous jump participates in solar ray tracing.

Absorptivity

contains the settings that define the absorptivity of the porous jump.

Direct Visible

specifies a multiplier (ranging from  to ) that is applied to the visible portion of the direct solar

radiation spectrum to account for the absorption of the porous jump.

Direct IR

specifies a multiplier (ranging from  to ) that is applied to the infrared portion of the direct

solar radiation spectrum to account for the absorption of the porous jump.

Transmissivity

contains the settings that define the transmissivity of the porous jump.

radiation spectrum to account for the transmissivity of the porous jump.

Direct IR

solar radiation spectrum to account for the transmissivity of the porous jump.

The Pressure Far-Field dialog box sets the boundary conditions for a pressure far-field zone. It is

opened from the Boundary Conditions Task Page (p. ). See Inputs at Pressure Far-Field Boundar-

Controls

Zone Name

Momentum

sets the far-field gauge static pressure.

sets the far-field Mach number.The Mach number can be subsonic, sonic, or supersonic.

allows you to select a Cartesian, Cylindrical, or Local Cylindrical coordinate system.This option is

available only for 3D geometry.

set the far-field flow direction.These items will appear if the selected Coordinate System is Cartesian

or the model is 2D non-axisymmetric.

set the far-field flow direction.These items will appear for 2D axisymmetric cases, or for 3D cases for

which the selected Coordinate System is Cylindrical or Local Cylindrical.

Viscosity Ratio as the Turbulence Specification Method.

Thermal

sets the far-field static temperature.

Radiation

contains the boundary conditions for the radiation model at the pressure far-field zone.

specifies whether or not the pressure far-field zone participates in solar ray tracing.

through the pressure far-field zone.

specifies whether or not the pressure far-field zone participates in the view factor calculation as part

of the S2S radiation model.This parameter is available only if you select the Surface to Surface radi-

Species

UDS

DPM

reflect

trap

trap

escape

wall-jet

The Pressure Inlet dialog box sets the boundary conditions for a pressure inlet zone. It is opened from

the Boundary Conditions Task Page (p. ). See Inputs at Pressure Inlet Boundaries (p. ) for details

Controls

Zone Name

Momentum

specifies the reference frame for the pressure inlet. If the cell zone adjacent to the pressure inlet is

moving, you can choose to specify the total temperature, total pressure, and velocity components

as Relative to Adjacent CellZone or Absolute in the Reference Frame drop-down list.

to compute initial values for pressure, temperature, and velocity if the pressure inlet boundary condition

quired.You also have the option to enable Prevent Reverse Flow. See Defining the Flow Direc-

tion (p. ) for information on specifying flow direction.

Radial-, Axial-Component of Flow Direction,Tangential-Velocity

Prevent Reverse Flow

Enables Fluent to erect artificial walls on the boundary mesh faces to prevent flow out of the domain.

The artificial walls are removed when the flow is no longer leaving the domain and when a favorable

pressure gradient is recovered at the boundary mesh faces.

Fluctuating Velocity Algorithm

(only available for transient cases where scale-resolving turbulence models such as SAS, DES, and LES

are enabled)

The following methods are available:

Synthetic Turbulence Generator

For details, see Inlet Boundary Conditions for Scale Resolving Simulations in the Fluent Theory

Guide.

Satisfy Mass Conservation?

(only available for the Vortex Method)

For details, see Vortex Method in the Fluent Theory Guide.

Off

Impedance

Thermal

Radiation

contains the boundary conditions for the radiation model at the pressure inlet.

specifies whether or not the pressure inlet participates in solar ray tracing.

through the pressure inlet.

specifies whether or not the pressure inlet participates in the view factor calculation as part of the

model.

Species

DPM

reflect

reflect

trap

escape

wall-jet

Potential

Potential

Box (p. ).

UDS

The Pressure Outlet dialog box sets the boundary conditions for a pressure outlet zone. It is opened

from the Boundary Conditions Task Page (p. ). See Inputs at Pressure Outlet Boundaries (p. ) for

Controls

Zone Name

Momentum

sets the gauge pressure at the outflow boundary.

sets a factor by which the Gauge Pressure is multiplied.This is provided mainly for cases where a

non-uniform distribution of the static pressure at the pressure outlet boundary is specified by means

of a profile file or a user-defined function.

sets the direction of the inflow stream should the flow reverse direction. If you choose Direction

Vector, you will define the flow direction components, and if you choose Normal to Boundary or

From Neighboring Cell, no inputs are required.You also have the option to enable Prevent Reverse

Flow. See Inputs at Pressure Outlet Boundaries (p. ) for information on specifying flow direction.

specifies how the pressure is calculated under backflow conditions.When the NRBC option is not

enabled, if you select Static Pressure, the Gauge Pressure is directly imposed as the boundary face

pressure; if you select Total Pressure, the Gauge Pressure will be combined with a dynamic contri-

bution that is based on the velocity in the adjacent cell zone. For NRBCs, if you select Static Pressure,

the Gauge Pressure is directly imposed as the pressure at infinity; if you select Total Pressure, the

pressure at infinity is a calculated value that is based on the Gauge Pressure.

Radial Equilibrium Pressure Distribution

enables the radial equilibrium pressure distribution. See Defining Static Pressure (p. ) for details.

This item appears only for 3D and axisymmetric swirl solvers.

Average Pressure Specification

allows the pressure along the outlet boundary to vary, but maintain an average equivalent to the

specified value in the Gauge Pressure input field. In this boundary implementation, the pressure

variation provides a low level of non-reflectivity. For more details, see Calculation Procedure at Pressure

Outlet Boundaries (p. ).

Note

The Average Pressure Specification option is not available if the Radial Equilibrium

Pressure Distribution option is enabled.

Target Mass Flow Rate

allows you to set mass flow rate as a boundary condition at the outlet.

Target Mass Flow

allows you to specify the flow as either a constant value or a user-defined function.

Upper Limit of Absolute Pressure, Lower Limit of Absolute Pressure

specifies the range of the pressure limits, which have different pressure variations on different

boundaries.The upper and lower pressure limits can be specified as a constant or a profile.

Off

Off

Impedance

Non Reflecting Parameters

contains settings for the non-reflecting boundary condition treatment.

Exit Pressure Specification

defines how the pressure is calculated. For Pressure at Infinity, the pressure at the boundary

relaxes toward the Gauge Pressure at infinity; for Average Boundary Pressure, an effort is made

to force the average pressure on the boundary to approach the Gauge Pressure value.

Thermal

Radiation

contains the boundary conditions for the radiation model at the pressure outlet.

specifies whether or not the pressure outlet participates in solar ray tracing.

through the pressure outlet.

specifies whether or not the pressure outlet participates in the view factor calculation as part of the

model.

Species

DPM

reflect

trap

escape

wall-jet

motion of the particles.This option is available only for a granular phase with the Mixture and Eulerian

This control is not available for the open channel VOF submodel.

(VOF model only) enables the open-channel flow boundary condition. See Modeling Open Channel

Flows (p. ) for more information.This option is available only when the Open Channel VOF sub-

model is selected in the Multiphase Model dialog box. Once you select this option, you can specify

the following conditions:

Outlet Group ID

is used to identify the different outlets that are part of the same outlet group. See Setting the

Outlet Group (p. ) for details.

Pressure Specification Method

specifies which method will be used to define the boundary conditions at the open-channel

pressure outlet.You can choose from the following options:

Refer to Pressure Outlet in the Fluent Theory Guide for more details.

Secondary Phase for Level Specification

allows you to choose the desired secondary phase.This control is available only for flow applications

with more than two phases.

can be determined by using the absolute value of height from the free surface to the origin in

the direction of gravity and applying the correct sign based on whether the free surface level is

above (positive) or below (negative) the origin. See Determining the Free Surface Level (p. )

is used for calculating the liquid height. It can be determined as described in Determining the

Bottom Level (p. ).

Density Interpolation Method

allows you to specify whether the mixture density used in the hydrostatic profile will be interpol-

ated using the From Neighboring Cell, From Free Surface Level, or Hybrid method. See

Choosing the Density Interpolation Method (p. ) for more information.This drop-down list is

available for sub-critical two-phase flow applications.

Potential

Box (p. ).

Box (p. ).

UDS

The Radiator dialog box sets the boundary conditions for a radiator model zone. It is opened from

the Boundary Conditions Task Page (p. ). See User Inputs for Radiators (p. ) for details about the

Controls

Zone Name

Loss Coefficient

specifies the loss coefficient as a constant value or as a polynomial, piecewise-linear, or piecewise-poly-

nomial function of velocity. See Defining the Pressure Loss Coefficient Function (p. ) for details.

specifies the heat-transfer coefficient as a constant value or as a polynomial, piecewise-linear, or piecewise-

polynomial function of velocity. See Defining the Heat Flux Parameters (p. ) for details.

sets the temperature used to compute heat flux from the radiator using the Heat-Transfer-Coefficient.

If Temperature is absolute zero, the Heat Flux condition is used instead.

Heat Flux

Heat Flux

sets the heat flux at the radiator surface (used only when Temperature is absolute zero).

interior

reflect

trap

escape

wall-jet

The RANS/LES Interface dialog box can be used to create artificial resolved turbulence (fluctuation/per-

turbations) at the interface where the flow proceeds from the RANS zone into the LES zone of the

computational domain for Embedded LES turbulent flows. It is opened from the Boundary Conditions

Task Page (p. ). See Setting Up the Embedded Large Eddy Simulation (ELES) Model (p. ) for more

information about RANS/LES interfaces.

Controls

Zone Name

sets the name of the RANS/LES interface.

displays the methods for generating fluctuating velocity components at the RANS/LES interface. Available

options include:

Number of Vortices

displays the amount of vortices that the selected fluctuating velocity method distributes randomly

over the face zone and uses to generate turbulent fluctuations (available for the Vortex Method

only).

Important

The RANS/LES 'interface' can either be an interior zone (that has been assigned to

be a rans-les-interface zone), or it can be a non-conformal interface. If it is a non-

conformal interface, then you need to identify the name of the non-conformal in-

terface's "interior" zone (for example, using the Mesh Interfaces Dialog Box (p. )),

and then go to that zone in the Boundary Conditions task page.

The Symmetry dialog box can be used to modify the name of a symmetry zone; there are no conditions

to be set. It is opened from the Boundary Conditions Task Page (p. ). See Symmetry Boundary

Conditions (p. ) for information about symmetry boundaries.

Controls

Controls

Zone Name

Phase

displays the name of the phase.This item is available only for multiphase flows.

The Velocity Inlet dialog box sets the boundary conditions for a velocity inlet zone. It is opened from

the Boundary Conditions Task Page (p. ). See Inputs at Velocity Inlet Boundaries (p. ) for details

Controls

Zone Name

Phase

allows you to set specific parameters for a particular boundary for open channel wave boundaries.This

is available when the volume of fluid multiphase model is selected.

Momentum

Velocity Specification Method

sets the method used to define the inflow velocity.

Flow Direction Specification Method

sets the method used to define the direction of flow of the wave.This is available when you enable

the Open Channel Wave BC option.

allows specification in terms of a Velocity Magnitude and Flow-Direction.

allows specification in terms of the Cartesian, cylindrical, or local cylindrical velocity components.

Magnitude, Normal to Boundary

allows specification of a Velocity Magnitude normal to the boundary.

specifies relative or absolute velocity inputs.You can choose to enter Absolute velocities or velocities

Relative to Adjacent Cell Zone. If you are not using moving reference frames, both options are

equivalent, so you need not choose.

Uniform Flow Velocity Magnitude

is the flow velocity, specified as a constant or a parameter.

specifies whether Cartesian, Cylindrical, or Local Cylindrical velocities will be defined.This item

will appear only for 3D cases in which you have selected Magnitude and Direction or Components

as the Velocity Specification Method.

X-,Y-, Z-Velocity

set the components of the velocity vector at the inflow boundary.These items will appear for 2D non-

axisymmetric models, or for 3D models if you select the Components option as the Velocity Specific-

ation Method and Cartesian as the Coordinate System.

Radial-,Tangential-, Axial-Velocity

set the components of the velocity vector at the inflow boundary.These items will appear for 3D

models if you select the Components option as the Velocity Specification Method and Cylindrical

or Local Cylindrical as the Coordinate System.

Axial-, Radial-, Swirl-Velocity

set the components of the velocity vector at the inflow boundary.These items will appear for 2D

axisymmetric models.

Important

Swirl-Velocity will appear only for 2D axisymmetric swirl models.

Angular Velocity

specifies the angular velocity  for a 3D flow.This item will appear for a 3D model if you select the

Components option as the Velocity Specification Method and Cylindrical or Local Cylindrical as

the Coordinate System.

Swirl Angular Velocity

specifies the swirl angular velocity  for an axisymmetric swirling flow.This item will appear for an

axisymmetric swirl model if you choose Components as the Velocity Specification Method.

sets the magnitude of the velocity vector at the inflow boundary.This item will appear if you select

the Magnitude and Direction or Magnitude, Normal to Boundary option as the Velocity Specific-

ation Method.

set the direction of the velocity vector at the inflow boundary.These items will appear for 2D non-

axisymmetric models if you select the Magnitude and Direction option as the Velocity Specification

Method, or for 3D models if you select the Magnitude and Direction option as the Velocity Specific-

set the direction of the velocity vector at the inlet boundary.These items will appear for 3D models

if you select the Magnitude and Direction option as the Velocity Specification Method and Cyl-

indrical or Local Cylindrical as the Coordinate System, or for 2D axisymmetric models.

Important

Tangential-Velocity will appear only for 2D axisymmetric swirl models.

specifies the pressure to be used as the pressure outlet condition if flow exits the domain at any face

on the velocity inlet boundary. (Note that this effect is similar to that of the “velocity far-field”

boundary that was available in RAMPANT .)

This item appears only for the density-based solvers.

Guide.

sets the value of the turbulence intensity  for the LES model.

Off

Impedance

Thermal

specifies the static temperature of the flow.

Radiation

contains the boundary conditions for the radiation model at the velocity inlet.

Radiation

specifies whether or not the velocity inlet participates in solar ray tracing.

through the velocity inlet.

specifies whether or not the velocity inlet participates in the view factor calculation as part of the S2S

Species

set inlet values for the PDF mixture fraction and its variance.These items will appear only if you are

using the non-premixed or partially premixed combustion model.

DPM

reflect

trap

escape

wall-jet

wall-jet

specifies the secondary phase to which the parameters are applied. In case of a three-phase flow,

select the corresponding secondary phase from this list.

Wave BC Options

allows you to choose between Shallow Waves, Shallow/Intermediate Waves or Short Gravity

Waves. Information about the two types of waves is available in Open Channel Wave Boundary

Conditions in the Theory Guide.

is determined by using the absolute value of height from the free surface to the origin in the direction

of gravity and applying the correct sign based on whether the free surface level is above (positive)

or below (negative) the origin.

is valid for shallow and intermediate waves.The bottom level is used for calculating the liquid height.

Reference Wave Direction

is the direction of wave propagation for a zero wave heading angle.

Wave Modeling Options

determines whether to use wave theory or a wave spectrum to model waves in the shallow/interme-

diate and short gravity wave regimes.

specifies the number of waves you are defining when modeling waves using wave theory.

allows you to choose from First Order Airy (the default), Second Order Stokes, Third Order Stokes,

Fourth Order Stokes, and Fifth Order Stokes for shallow/intermediate waves and short gravity

waves. For shallow waves, you can choose between Fifth Order Solitary and Fifth Order Cnoidal.

Information about the types of wave theory is available in Open Channel Wave Boundary Conditions

Since a solitary wave does not have troughs, the wave height is the distance between a wave

crest to mean free surface level.

is the wave length of the shallow wave or short gravity wave.

This option is used to generate a wave from a location other than the reference frame origin.

is the phase difference between one wave and another.

is the angle between the direction of the wavefront and the reference wave direction, in the plane

of the flow surface. In 2D, there are only two possibilities, zero degrees when the wave is in the refer-

ence wave direction, and  degrees when the wave is in the opposite direction.

specifies the spectrum to use.You can select Pierson-Moskowitz (appropriate for fully-developed

seas), Jonswap (appropriate for fetch-limited seas), or TMA (appropriate for fetch-limited, finite-depth

seas).

in Equa-

tion . and Equation . in the Fluent Theory Guide.

can be expressed in terms of the peak

wave period,

, as

.

specify the frequency range for the spectrum. Note that the Peak Wave Frequency must fall in

between Minimum Wave Frequency and Maximum Wave Frequency.

specifies the method to use for specifying the directional spreading characteristics.You can choose

Unidirectional (for long-crested waves), Frequency Independent Cosine Function (for short-crested

waves where the directional component does not depend on frequency), and Frequency Dependant

Hyperbolic Function (for short-crested waves where the directional component depends on fre-

quency).

quency).

specifies the exponent in the Frequency Independent Cosine Function formulation.This corresponds

to  in Equation . in the Fluent Theory Guide.

Potential

Box (p. ).

UDS

The Wall dialog box sets the boundary conditions for a wall zone. It is opened from the Boundary

Conditions Task Page (p. ). See Inputs at Wall Boundaries (p. ) for details about defining the items

below.

Controls

Zone Name

below.

Controls

Zone Name

Phase

Adjacent Cell Zone

shows the name of the cell zone adjacent to the wall. (This is for informational use only; you cannot edit

this field.)

Interface Zone

displays the name of the associated interface zone.This field appears if this wall zone was created as a

non-overlapping zone during the creation of a mesh interface. It is for informational use only; you cannot

edit this field.

Momentum

Wall Motion

contains options for specifying whether or not the wall is moving.

Stationary Wall

specifies that the wall is not moving relative to the adjacent cell zone.

Moving Wall

enables specification of the tangential wall motion.Tangential wall motion is applicable only to

viscous flows. Since the inviscid slip condition decouples the tangential wall velocity from the

governing equations, tangential wall motion has no effect on inviscid flow.

Motion

contains inputs related to wall motion. See Velocity Conditions for Moving Walls (p. ) for details.

Relative to Adjacent Cell Zone

enables the specification of a wall velocity relative to the velocity of the adjacent cell zone. (If the

adjacent cell zone is not moving, this is equivalent to Absolute.)

Absolute

enables the specification of an absolute wall velocity,

Translational

enables the specification of a translational wall velocity.

Rotational

enables the specification of a rotational wall velocity.

enables the specification of wall velocity components.

Speed

sets the translational or rotational speed of the wall (depending on whether you selected Trans-

lational or Rotational).

Direction

sets the direction vector of the translational velocity. (This item will appear if you have chosen

the Translational option.)

sets the coordinates of the origin of the axis of rotation, thereby determining the location of the

axis. (This item will appear if you have chosen the Rotational option for a non-axisymmetric case.)

sets the direction vector for the axis of rotation. (This item will appear if you have chosen the

Rotational option for a non-axisymmetric case.)

Velocity Components

sets the X, Y, and Z-Velocity components of the wall motion. (This item will appear if you have

chosen the Components option.)

Shear Condition

contains options for specifying the shear conditions at the wall.

No Slip

specifies a no-slip condition at the wall. No further inputs are required.

Specified Shear

enables specification of zero or nonzero shear. See Specified Shear (p. ) for details.This option

is not available for moving walls.

Marangoni Stress

enables the specification of shear stress caused by the variation of surface tension due to temper-

ature.This option is not available for moving walls.

Shear Stress

contains inputs related to wall shear.These items will appear when Specified Shear is selected as

the Shear Condition. See Specified Shear (p. ) for details.

X-Component,Y-Component, Z-Component, Swirl Component

specify the ,

, and  or swirl components of shear for a slip wall. Swirl Component is available

only for axisymmetric swirl cases.

Specularity Coefficient

is used in multiphase granular flow.You can specify the specularity coefficient such that when the

value is zero, this condition is equivalent to zero shear at the wall, but when the value is near unity,

there is a significant amount of lateral momentum transfer.

allows you to enter a value between zero and one, which controls the amount of lateral momentum

transfer.

contains inputs related to Marangoni stress.This item will appear when Marangoni Stress is selected

as the Shear Condition. See Marangoni Stress (p. ) for details.

Surface Tension Gradient

specifies the surface tension gradient with respect to temperature (

in Equa-

Wall Roughness

contains various models for defining wall roughness size/height in turbulent calculations.

Standard

uses the standard wall roughness methods for most turbulence models. See Wall Roughness Effects

in Turbulent Wall-Bounded Flows (p. ) for details.

High Roughness (Icing)

contains various models for use only with the Spalart-Allmaras and SST k-ω turbulence models.

Specifically applicable to icing simulations, choose from Specified Roughness, NASA Correlation,

Shin-et-al, or ICE3D Roughness File methods to specify the Sand-Grain Roughness. See Addi-

tional Roughness Models for Icing Simulations (p. ) for details.

contains inputs related to wall adhesion.This section of the dialog box will appear if you are using

the VOF model and have enabled wall adhesion in the e Phase Interaction Dialog Box (p. ).

Contact Angles

specifies the contact angle at the wall for each pair of phases (

in Figure . : Measuring the

Contact Angle (p. ) in the Theory Guide). See Steps for Setting Boundary Conditions (p. ) for

details.

Thermal

contains the thermal parameters.This tab is available only when the energy equation is turned on.

Thermal Conditions

contains radio buttons for selecting the thermal boundary condition type. See Thermal Boundary

Conditions at Walls (p. ) for details about these inputs:

Heat Flux

selects a specified heat flux condition.

selects a specified wall temperature condition.

Convection

selects a convective heat transfer boundary condition model.

Radiation

selects an external radiation boundary condition.

Mixed

selects a combined convection/external radiation boundary condition.

Coupled

selects a coupled heat transfer condition. It is applicable only to walls that form the interface

between two regions (such as the fluid/solid interface for a conjugate heat transfer problem).

via System Coupling

selects a heat transfer condition where a boundary can receive thermal data (either wall temper-

ature or heat flow) from the System Coupling service. It is applicable when ANSYS Fluent is coupled

with another system in Workbench using System Coupling (see Heat Transfer Boundary Conditions

Through System Coupling (p. ) for details).

via Mapped Interface

specifies that the thermal data is interpolated across a mapped interface. It is available only for

the interface wall boundary zones created as part of a mapped interface (see Heat Transfer

Boundary Conditions Across a Mapped Interface (p. ) for details).

Once a condition type has been selected, the appropriate conditions can be specified.

Heat Flux

sets the wall heat flux to be used for the Heat Flux condition. A specification of zero Heat Flux is

simply the adiabatic condition (no heat transfer). A positive value of heat flux implies that heat enters

into the domain.

sets the wall temperature to be used for the Temperature condition.

sets the convective heat transfer coefficient to be used for the Convection condition (

in Equa-

Free Stream Temperature

sets the reference or free stream temperature to be used for the Convection condition (

in

Equation . (p. )).

External Emissivity

sets the emissivity of the external wall to be used for the Radiation condition (

in Equa-

External Radiation Temperature

sets the temperature of the external radiation source/sink to be used for the Radiation condition

(

Internal Emissivity

sets the internal emissivity of the wall.This item will appear only if you are using the gray P-, DO,

MC, DTRM, or S2S models for radiation heat transfer. (Note that it will not appear if you are using the

non-gray P-, DO, or MC model. In these cases, you will enter the Internal Emissivity for each band

in the Radiation tab.)

Wall Thickness

sets the thickness of a thin wall for the calculation of thermal resistance. (See Thin-Wall Thermal Res-

istance Parameters (p. ) for details.)

Heat Generation Rate

sets the rate of heat generation in a wall without shell conduction.

Contact Resistance

sets the contact resistance (

in Equation . in the Theory Guide) at the wall. See Modeling Solid-

ification and Melting (p. ) for details.This item appears only when the solidification/melting model

is used.

sets the material type for a thin wall.The conductivity of the material is used for the calculation of

thin-wall thermal resistance. (See Thin-Wall Thermal Resistance Parameters (p. ) for details.) Mater-

ial is used only when Wall Thickness is nonzero. Materials are defined with the Materials Task

Page (p. ).

Shell Conduction

enables shell conduction for the wall. See Shell Conduction (p. ) for details.

Edit...

is only available when Shell Conduction is enabled, and opens the Shell Conduction Layers Dialog

Box (p. ) in order to allow you to define the shell conduction settings for the wall.

Radiation

displays the boundary conditions for the S2S model, the DO model, the MC model, and the non-gray P-

model at the wall.This tab is only available if you are using the surface to surface model, the discrete

ordinates model, the Monte Carlo model, or the non-gray P- model. See Forming Surface Clusters (p. ),

Wall Boundary Conditions for the DO Model (p. ), and Wall Boundary Conditions for the DTRM, and the

P-, S2S, and Rosseland Models (p. ) for details.

BC Type

BC Type

contains a drop-down list of available radiation boundary condition types.The available options are

opaque and semi-transparent.This item will appear only if you are using the discrete ordinates or

Monte Carlo model.

Boundary Source

enables the wall to be an external radiation source.This is only available for the MC model or with

semi-transparent walls for the DO model.

Polar Distribution Function

enables a polar (rotationally symmetric about a given direction) boundary source which can be used

if the irradiation intensity varies with direction such as in the case of LED light sources.The polar

distribution function is defined by an Expression or by a table of data pairs consisting of an Angle

and it's corresponding Relative Intensity.You have the option to read and write the polar data in

the form of .csv files or plotting the data in the graphics window. Only available with the MC model.

Reference Direction

Specify the (X,Y,Z) vector that defines the center of the polar distribution function. Only available with

the MC model.

specifies the internal emissivity of the wall in each wavelength band.This item will appear only if you

are using the non-gray discrete ordinates or Monte Carlo models and you have selected opaque as

the BC Type, or if you are using the non-gray P- model.

Diffuse Fraction

specifies the fraction of the irradiation that is to be treated as diffuse. By default, the Diffuse Fraction

is set to , indicating that all of the irradiation is diffuse. If the non-gray DO or MC model is being

used, the Diffuse Fraction can be specified for each band.This item will appear only if you are using

the Monte Carlo or discrete ordinates model.

Beam Width

specifies the beam width for an external semi-transparent wall in terms of the Theta and Phi extents.

This item will appear only if you are using the discrete ordinates radiation model and you have selected

semi-transparent as the BC Type.

Beam Direction

specifies the beam direction as an X,Y,Z vector.You can specify the Beam Direction as a constant,

a profile, or a user-defined function.This item will appear only if you are using the Monte Carlo

model or the discrete ordinates radiation model and you have selected semi-transparent as the BC

Type.

Direct Irradiation

specifies the value of the irradiation flux. If the non-gray DO or MC models are being used, a constant

Direct Irradiation can be specified for each band.

This item will appear only if you are using the semi-transparent BC Type with the discrete

ordinates radiation model.

Apply Direct Irradiation Parallel to the Beam

is the default means of specifying the scale of irradiation flux.When enabled, ANSYS Fluent assumes

that the value of Direct Irradiation that you specify is the irradiation flux parallel to the Beam Direc-

tion.When deselected, ANSYS Fluent instead assumes that the value specified is the flux parallel to

the face normals and will calculate the resulting beam parallel flux for every face.This item will appear

only if you are using the discrete ordinates model.

Diffuse Irradiation

specifies the value of the irradiation flux. If the non-gray DO model is being used, a constant Diffuse

Irradiation can be specified for each band.

This item will appear only if you are using the discrete ordinates radiation model and you have

selected semi-transparent as the BC Type.

contains the settings for solar ray tracing.This group box is available only if you select Solar Ray

Tracing from the Model list in the Solar Load group box of the Radiation Model dialog box. For

semitransparent coupled walls, the solar ray tracing settings are defined on the original wall and not

on the shadow wall. See Solar Ray Tracing (p. ) for details.

specifies whether or not the wall participates in solar ray tracing.

contains the settings that define the absorptivity of wall.

specifies a multiplier (ranging from  to ) that is applied to the visible portion of the direct

solar radiation spectrum to account for the absorption of the wall.The value should be defined

for normal incident rays.

Direct IR

Diffuse Hemispherical

specifies a multiplier (ranging from  to ) that is applied to the diffuse solar radiation to ac-

count for the absorption of the wall.This setting is only available for semi-transparent walls.

contains the settings that define the transmissivity of wall.This group box is only available when

semi-transparent is selected for BC Type.

solar radiation spectrum to account for the transmissivity of the wall.The value should be

defined for normal incident rays.This setting is only available for semi-transparent walls.

Direct IR

specifies a multiplier (ranging from  to ) that is applied to the diffuse solar irradiation to

account for the transmissivity of the wall.This setting is only available for semi-transparent

walls.

S2S Parameters

contains the settings for the S2S radiation model.This group box is available only if you select the

Surface to Surface radiation model. See Forming Surface Clusters (p. ) for details.

Faces Per Surface Cluster

sets the number of faces per surface cluster (FPSC) for the wall, and thus controls the number of

radiating surfaces and (if you select Cluster to Cluster for Basis in the View Factors and Clustering

dialog box) view factor surfaces.

Critical Zone

specifies that the wall is a critical zone.When this option is enabled, the value entered for Faces

Per Surface Cluster will not be altered when you use Automatic clustering in the View Factors

and Clustering dialog box, and impacts the calculations and actions performed by the buttons

in the Maximum Distance from Critical Zone group box of the Participating Boundary Zones

specifies whether or not the wall participates in the view factor calculation as part of the S2S ra-

diation model.This option is available only if you select the Surface to Surface radiation model.

Species

contains the species parameters.This tab is available only if you have enabled the Species Transport

model in the Species Model Dialog Box (p. ).

Reaction

activates reactions at the wall.This item will appear only if you have enabled any of the reactions in

the Species Model Dialog Box (p. ).

Reaction Mechanisms

allows you to specify a defined group, or mechanism, of available reactions.This item will appear only

if the Reaction option has been turned on. See Defining Zone-Based Reaction Mechanisms (p. )

for details about defining reaction mechanisms.

Surface Area Washcoat Factor

allows you to specify a factor, which multiplies the wall area to account for the increased surface area

of washcoats.This item will appear only if the Reaction option has been turned on. See Species

Boundary Conditions for Walls (p. ) for details.

Species Boundary Condition

contains options for the specification of species boundary conditions. See Species Boundary Conditions

for Walls (p. ) for details.

Zero Diffusive Flux

indicates a zero-flux condition for a species.This is the default condition.

Specified Mass Fraction

indicates that the species mass fraction will be specified.

contains inputs for the species mass fractions of any species for which you have selected Species

Mass Fraction as the Species Boundary Condition.

DPM

Discrete Phase Model Conditions

contains inputs for setting the fate of particle trajectories at the wall.These options will appear when

one or more injections have been defined. See Setting Boundary Conditions for the Discrete

Boundary Cond.Type

sets the way that the discrete phase behaves with respect to the boundary.

reflect

rebounds the particle off the boundary with a change in its momentum as defined by the

coefficients of restitution (see Particle Reflection at Wall in the Fluent Theory Guide).When at

least one injection accounts for the rough wall model (the Rough Wall Model option is selected

under the Physical Models tab in the Set Injections Properties dialog box), you can specify

the DPM Wall Roughness Parameters (Ra, Rq, and RSm in Equation . in the Fluent

Theory Guide). (See Rough Wall Model (p. )).

trap

terminates the trajectory calculations and records the fate of the particle as “trapped”. In the

case of evaporating droplets, their entire mass instantaneously passes into the vapor phase

and enters the cell adjacent to the boundary. See Figure . :“Trap” Boundary Condition

for the Discrete Phase (p. ).

escape

reports the particle as having “escaped” when it encounters the boundary.Trajectory calcula-

escape

tions are terminated. See Figure . :“Escape” Boundary Condition for the Discrete

wall-jet

indicates that the direction and velocity of the droplet particles are given by the resulting

momentum flux, which is a function of the impingement angle. See Figure . :“Wall Jet”

Boundary Condition for the Discrete Phase in the Theory Guide.

wall-film

allows you to enable:

Particle-Wall Heat Exchange (Particle-Wall Impingement Heat Transfer (p. ))

Film Condensation (Film Condensation Model (p. ))

Wall Boundary Layer Model (Wall Boundary Layer Model (p. ))

and specify Impingement/Splashing Model Parameters, Separation Model Paramet-

ers, and parameters for Erosion Models (Setting Particle Erosion and Accretion Para-

meters (p. )).

See Discrete Phase Boundary Condition Types (p. ) for details about the wall-film

models and their parameters.

Boundary Cond. Function

Discrete Phase Reflection Coefficients

determine the behavior of reflecting particles.This item appears when reflect is chosen as the

Boundary Cond.Type. See Discrete Phase Boundary Condition Types (p. ) for details on setting

the following items.

Normal

sets the type of function for the normal coefficient of restitution.This function can be constant,

Normal

piecewise-linear, piecewise-polynomial, or polynomial.

Tangent

sets the type of function for the tangential coefficient of restitution.This function can be constant,

DEM Collision Partner

contains a list of names to designate the collision partner.

Erosion Model

contains a list of erosion models. See Setting Particle Erosion and Accretion Parameters (p. ) for

details about these items.

specifies erosion rates to be computed using the generic erosion model. (See Accretion in the

Fluent Theory Guide for background information about this model.) When this model is enabled,

you must specify the erosion parameters in the Generic Erosion Model Parameters dialog box

(opened by clicking the corresponding Edit… button) as described in Setting Particle Erosion

and Accretion Parameters (p. ).

Finnie

specifies erosion rates to be computed using the Finnie formulation. (See Accretion in the Fluent

Theory Guide for background information about this model.) When this model is enabled, you

must specify the erosion parameters in the Finnie Model Parameters dialog box (opened by

clicking the corresponding Edit… button) as described in Setting Particle Erosion and Accretion

McLaury

specifies erosion rates to be computed using the McLaury formulation. (See McLaury Erosion

Model in the Fluent Theory Guide for background information about this model.) When this model

is enabled, you must specify the erosion parameters in the McLaury Model Parameters dialog

box (opened by clicking the corresponding Edit… button) as described in Setting Particle Erosion

Oka

specifies erosion rates to be computed using the Oka formulation. (See Oka Erosion Model in the

you must specify the erosion parameters in the Oka Model Parameters dialog box (opened by

Sheer Stress

specifies erosion rates to be computed using the sheer stress model. (See Abrasive Erosion Caused

by Solid Particles in the Fluent Theory Guide for background information about this model.) When

this model is enabled, you must specify the erosion parameters in the Sheer Stress Model

Parameters dialog box (opened by clicking the corresponding Edit… button) as described in

Setting Particle Erosion and Accretion Parameters (p. ).This model is available only for multiphase

flow with a dispersed secondary granular phase.

Granular Phase Shielding

includes the shielding effect in other erosion models that are currently enabled.The granular

phase shielding is always considered in the sheer stress erosion model. (See Wall Shielding Effect

in Dense Flow Regimes in the Fluent Theory Guide for background information about this model.)

This option is available only when Shear Stress Model Parameters is selected.

Friction Coefficient

specifies  in Equation . and Equation . in the Fluent Theory Guide as a constant or a

piecewise-linear, piecewise-polynomial, or polynomial function of relative velocity.This item appears

only when Enable Rotation is selected under the Physical Model tab of the Set Injection Properties

UDS

displays the boundary conditions for user-defined scalars (UDSs) at the wall.This tab is available only if

you have specified a nonzero number of user-defined scalars in the User-Defined Scalars Dialog Box (p. ).

User Defined Scalar Boundary Condition

contains options for the specification of UDS boundary conditions. See the separate Fluent Custom-

ization Manual for details.

Specified Flux

indicates that the flux of the UDS at the wall will be specified.

Specified Value

indicates that the value for the UDS at the wall will be specified.

User Defined Scalar Boundary Value

contains inputs for the value of the flux of the UDS, or the value of the UDS itself, depending on your

selection for that UDS under User Defined Scalar Boundary Condition.

Wall Film

displays the boundary conditions for liquid films at the wall.This tab is available only if you have enabled

the Eulerian Wall Film model in the Models Task Page (p. ).

Eulerian Film Wall

allows you to define a film wall condition for any wall. See Modeling Eulerian Wall Films (p. ) for

details. Once this option is enabled, you can set the following:

Film Condition Type

allows you to select the desired condition type.

Boundary Condition

allows you to specify settings for boundary Film Conditions:

Film Mass Flux

The film mass source in terms of mass flux per unit area (kg/m2–s).

X-Momentum Flux,Y-Momentum Flux, and Z-Momentum Flux

The film momentum source in terms of momentum flux per unit area (N/m2).

Incoming Film Temperature

The film temperature (K).

Film Passive Scalar Flux

The film passive scalar source in terms of mass flux per unit area (kg/m2–s).

Initial Condition

allows you to specify settings for initial Film Conditions:

Film Height

The film height at the wall boundary.

X-Velocity,Y-Velocity, and Z-Velocity

The film velocity components at the wall boundary.

The film passive scalar at the wall boundary (dimensionless).

Relative Film Momentum Flux

(moving reference frames or moving walls only) enables specification of the film momentum flux

relative to the wall on which liquid film is defined (Boundary Condition type only).This option

is only available when Moving Wall is selected in the Wall dialog box and/or Frame Motion is

selected in the Fluid dialog box.

Relative Initial Film Velocity

(moving reference frames or moving walls only) enables specification of the initial velocity relative

to the wall on which liquid film is defined (Initial Condition type only).This option is only available

when Moving Wall is selected in the Wall dialog box and/or Frame Motion is selected in the

User Source Terms

enables you to specify the additional source terms to the film continuity (Mass Flux), momentum

(X-Momentum Flux, Y-Momentum Flux, and Z-Momentum Flux), energy (Heat Flux), and

passive scalar equations (Scalar Flux).This option is only available with initial conditions.

Flow Momentum Coupling

When this option is selected, the liquid film and the gas flow will share the same velocity at the

interface of the liquid-gas interface using a two-way coupling.When this option is not selected,

the coupling between the liquid film and the gas flow is only one-way, namely, while the gas flow

impacts the film flow, the film flow does not impact the bulk of the gas flow.

Film Phase Change

enables the phase change for the selected wall.This option is available only when Phase Change

is selected in the Model Options and Setup tab of the Eulerian Wall Film Dialog Box (p. ). Once

enabled, you can select Phase Change Model and specify its parameters (in the Phase Change

Parameters group box).The following models are available:

diffusion-balance:You can specify Condensation Constant and Vaporization Constant.

wall-boundary-layer: No user input is required.

user-defined:You can specify Condensation Rate and Vaporization Rate as constants,

parameters, or profile user-defined functions (UDFs). Note that condensation and vaporization

rates must be specified as positive values in kg/s. For more information on profile UDFs, the

separate Fluent Customization Manual.

For more information on the phase change models see Coupling of Wall Film with Mixture

Species Transport in the Fluent Theory Guide.

Film Contact Angle

enables the Partial Wetting model.This option is available only with initial condition when Surface

Tension is selected in the Model Options and Setup tab of the Eulerian Wall Film Dialog

Box (p. ). Once this option is enabled, you can specify the Contact Angle Parameters:

Contact Angle: Is

described in Partial Wetting Effect in the Fluent Theory Guide.The input

range for this parameter is  to  degrees.

Relative Standard Deviation: Is  described in Partial Wetting Effect in the Fluent Theory Guide.

Contact Angle Force Beta: Is  in Equation . in the Fluent Theory Guide.The input range

for this parameter is  to .

For more information on modelling film partial wetting effect see Partial Wetting Effect in

Impingement Parameters

contains parameters related to particle-wall impingement

is a drop-down list that contains available impingement models:

stanton-rutland (default): consists of four impingement regimes: stick, rebound, spread

and splash, which are based on the impact energy and wall temperature. See The Stanton-

Rutland Model in the Fluent Theory Guide for details.

kuhnke: consists of four impingement regimes: stick, rebound, spread and splash (thermal

breakup). See The Kuhnke Model in the Fluent Theory Guide for details.

DPM Wall Splash

allows you to enable the wall splashing for the selected wall and specify the Number of

Splashed Particles.The minimum value is .This option is available when Particle Splashing

is enabled in the Eulerian Wall Film dialog box.

Kuhnke Model Parameters

(available when the kuhnke model is selected from the Impingement Model drop-down list)

Wall Roughness Length

enables you to specify wall roughness values used by the Kuhnke model:

Ra: the wall mean roughness that is used to compute

Theory Guide

Rz: the average surface roughness that is used to compute splashed particle reflection

angle distribution Equation . in the Fluent Theory Guide.

Critical Temperature Factor

is the dimensionless variable that is used to determine the impingement regime transition

temperature in Equation . in the Fluent Theory Guide.

Potential

displays the boundary conditions for the electric potential field at the wall.This tab is available only if

you have enabled either the Electric Potential model under the Model tree branch or the Electrochem-

ical Reaction model in the Species Dialog Box (p. ).

Electrochemical Reaction

enables electrochemical reactions at the wall.This option is available only if Electrochemical reactions

are enabled in the Species Model dialog box.

Faradaic Heat

(if enabled) includes heat from the electrochemical reaction in the energy equation.This option is

available only if Electrochemical reactions are enabled in the Species Model dialog box.

contains a drop-down list of all available electrochemical reaction mechanisms.This option is available

only if Electrochemical reactions are enabled in the Species Model dialog box.

contains a drop-down list of available potential boundary condition types for the external wall.You

will need to specify one of the following:

Current Density (Select the Specified Flux potential boundary condition)

Potential at the wall (Select the Specified Value potential boundary condition)

This control is available only for one-sided external walls. For two-sided internal walls, the

solver always uses the coupled treatment.

is the contact resistance at the wall,

in Equation . in the Fluent Theory Guide. For two-sided in-

ternal walls, you only need to define the contact resistance at one of the walls.The value you specify

will be automatically copied to the other side of the wall.

Structure

contains the displacement boundary condition settings for walls that are adjacent to solid cell zones.This

tab is only available when a model is selected in the Structural Model Dialog Box (p. ).

X-Displacement Boundary Condition,Y-Displacement Boundary Condition, Z-Displacement

contains a drop-down list of methods for calculating the displacement of the nodes in that particular

direction:

Node X-, Node Y-, and (for 3D cases) Node Z-Force specifies that the displacement results from a

specified force applied on the nodes, which is defined using the Node X-, Node Y-, and (for 3D

cases) Node Z-Force field.

Node X-, Node Y-, and (for 3D cases) Node Z-Displacement applies a specified displacement on

the nodes, which is defined using the X-, Y-, and (for 3D cases) Z-Displacement field.

Face Pressure specifies that the displacement results from a specified pressure load on the faces,

which is defined using the Face Pressure field.

Intrinsic FSI specifies that the displacement results from pressure loads exerted by the fluid flow

on the faces. Note that this selection is only available for a zone that is part of a wall / wall-shadow

pair.

The Periodic Conditions dialog box allows you to set parameters that define fully-developed periodic

flow and heat transfer. See User Inputs for the Pressure-Based Solver (p. ) and Using Periodic Heat

Transfer (p. ) for details.

(This dialog box is available only when the pressure-based solver is used; it is not available for the

density-based coupled solvers.)

Controls

Specify Mass Flow

enables the specification of the mass flow rate.

Specify Pressure Gradient

enables the specification of the pressure gradient.

specifies the mass flow rate.This item will not be available if you selected the Specify Pressure Gradient

option.

Important

radians.

specifies the pressure gradient (  in Equation . in the Theory Guide).

Upstream Bulk Temperature

sets the inlet bulk temperature for periodic heat transfer calculations.

sets the direction of the periodic flow.The direction vector must be parallel to the periodic translation

direction or its opposite.

Relaxation Factor

sets the under-relaxation factor that controls convergence of the iteration process described in Setting

Parameters for the Calculation of β (p. ) for specified mass flow.

sets the number of subiterations done on the correction of  in the pressure correction equation for

specified mass flow. See Setting Parameters for the Calculation of β (p. ) for details.

Update

updates the Pressure Gradient field with the current value.

The Overset Interfaces task page allows you to create overset interfaces. For additional information

about overset interfaces, see Overset Meshes (p. ).

Overset Interfaces Task Page

Controls

displays the Create/Edit Overset Interfaces Dialog Box (p. ).

displays the Mesh Motion Dialog Box (p. ).

... Create/Edit Overset Interfaces Dialog Box

The Create/Edit Overset Interfaces dialog box allows you to create and delete overset interfaces. For

additional information, see Overset Meshes (p. ).

Overset Interface

contains a text entry box where you must specify the name of the overset interface. Below is a list of all

existing overset interfaces.

Background Zones

lists all of the background zones available for selection when creating an overset interface. Multiple

background zones can be part of an overset interface; however, a background zone cannot be

part of multiple overset interfaces. It is acceptable to have an interface with only component zones

and no background zones.

Component Zones

lists all of the component zones available for selection when creating of an overset interface. Multiple

components can be part of an overset interface; however, a component zone cannot be part of multiple

overset interfaces.

Create

creates an overset interface using the name in the Overset Interface text box and the zones selected

under Background Zones and Component Zones. Note that grid priorities, if required, are added to the

interface after it is created, using the text command define/overset-interfaces/grid-prior-

ities.

Delete

deletes the selected Overset Interface.

Delete All

deletes all overset interfaces in the domain.

List

prints zonal information and grid priorities for the selected Overset Interface.

The Dynamic Mesh task page allows you to define the all the parameters for modeling a dynamic mesh

model. See Setting Dynamic Mesh Modeling Parameters (p. ) for details about using the items below.

Dynamic Mesh Task Page

Controls

enables the dynamic mesh model and activates the controls in the task page.

Mesh Methods

contains options to specify the mesh update method(s).

Smoothing

enables mesh smoothing. See Smoothing Methods (p. ) for details about the smoothing methods

Layering

enables the dynamic layering method that can be used to add or remove layers of cells adjacent to a

moving boundary based on the height of the layer adjacent to the moving surface in prismatic mesh

zones. See Dynamic Layering (p. ) for details.

Remeshing

enables the local or zonal remeshing methods. In local remeshing, the cells that violate the skewness

Remeshing

or size criteria are agglomerated and locally remeshed; see Local Remeshing Method (p. )  for further

details. In zonal remeshing, the complete cell zone (including the boundary zones) is remeshed; see

CutCell Zone Remeshing Method (p. ) for further details.

displays the Mesh Method Settings Dialog Box (p. ) in which you can specify settings for the

Smoothing, Layering, and Remeshing methods.

Options

contains options to specify specialized dynamic mesh models.

enables the in-cylinder model. See In-Cylinder Settings (p. ) for more information.

Six DOF

enables the six degrees of freedom (DOF) solver. See Six DOF Solver Settings (p. ) for more informa-

tion.

specifies that the mesh is updated during a time step (as opposed to just at the beginning of a time

step). See Implicit Update Settings (p. ) for more information.

Contact Detection

enables contact detection. See Contact Detection Settings (p. ) for more information.

opens the Options Dialog Box (p. ), where you can set the parameters for the options that are enabled

in the Options group box.

Events...

displays the Dynamic Mesh Events Dialog Box (p. ).

Dynamic Mesh Zones

displays a list of dynamic mesh zones.

displays the Dynamic Mesh Zones Dialog Box (p. ).

Delete

removes the selected dynamic zone(s) from the Dynamic Mesh Zones list.

Delete All

removes all dynamic zones from the Dynamic Mesh Zones list.

Display Zone Motion...

displays the Zone Motion Dialog Box (p. ).

... Mesh Method Settings Dialog Box

... Mesh Smoothing Parameters Dialog Box

... Mesh Scale Info Dialog Box

... Options Dialog Box

... In-Cylinder Output Controls Dialog Box

... Six DOF Properties Dialog Box

... Flow Controls Dialog Box

... Dynamic Mesh Events Dialog Box

... Define Event Dialog Box

... Events Preview Dialog Box

... Dynamic Mesh Zones Dialog Box

... Orientation Calculator Dialog Box

... Inflation Settings Dialog Box

... CutCell Boundary Zones Info Dialog Box

... Zone Scale Info Dialog Box

... Zone Motion Dialog Box

... Mesh Motion Dialog Box

... Autosave Case During Mesh Motion Preview Dialog Box

The Mesh Method Settings dialog box allows you to apply settings for the smoothing, layering, or

remeshing methods.

Controls

Smoothing

contains parameters to be specified for the smoothing mesh update method.

Method

allows you to specify the smoothing method.

Spring/Laplace/Boundary Layer

specifies that the smoothing method is spring based, or appropriate for the Laplacian smoothing

method (for .5D remeshing) or the boundary layer smoothing method.

Diffusion

selects the diffusion-based smoothing method.

Linearly Elastic Solid

selects smoothing based on the equations for a linearly elastic solid.

opens the Mesh Smoothing Parameters Dialog Box (p. ), in which you can define the settings for

the selected smoothing Method.

Layering

contains parameters to be specified for the layering mesh update method.

Options

Layering

Options

specifies the criteria for splitting or collapsing cell layers.

Height Based

specifies that the cell layers are split or merged based on height.

Ratio Based

specifies that the cell layers are split or merged based on ratios.

Split Factor

in Equation . (p. ). It controls the height or ratio at which the cells are

split.

Collapse Factor

collapsed and merged into the next layer.

Remeshing

contains parameters to be specified for the remeshing mesh update method.

Remeshing Methods

contain options that control remeshing.

Local Cell

allows you to remesh deforming boundary cells.

Local Face

allows you to remesh deforming boundary faces.This option is available for 3D cases.

Region Face

allows you to remesh a region.

CutCell Zone

allows you to replace an entire cell zone with a predominantly Cartesian mesh.This option is only

available for 3D cases. Note that the parameters that control this remeshing method are set in

the Dynamic Mesh Zones dialog box. See Using the CutCell Zone Remeshing Method (p. ) for

.5D

enables the .5D model.This option is only available for 3D cases. See Using the .5D Model (p. )

contains parameters that control remeshing for all of the remeshing methods except for CutCell

Zone.

Minimum Length Scale

specifies the lower limit of cell size below which the cells are marked for remeshing.

Maximum Length Scale

specifies the upper limit of cell size above which the cells are marked for remeshing.

Maximum Cell Skewness

specifies the desired maximum skewness for the mesh.

Maximum Face Skewness

specifies the desired maximum skewness for the surface mesh.This option is active, when Local

Face is selected under Remeshing Methods.

Size Remeshing Interval

specifies the interval in time steps for remeshing based on the above size criteria only. Marking

of cells based on skewness occurs automatically at every time step when Remeshing is enabled.

Mesh Scale Info...

opens the Mesh Scale Info Dialog Box (p. ), in which you can view the statistics of the mesh,

such as the minimum and maximum length scale values and the maximum cell and face skewness

values.

Default

sets the fields in the Parameters group box to values that represent a reasonable starting point

for your particular mesh, as determined by ANSYS Fluent. After execution, the Default button

becomes the Reset button.

Reset

resets the fields in the Parameters group box to the prior values (that is, those displayed at the

moment the Default button was clicked). After execution, the Reset button becomes the Default

button.

Sizing Options

contains parameters that control the sizing function.

Sizing Function

allows you to enable or disable the sizing function.

sets the resolution for the sizing function. See Setting Dynamic Mesh Modeling Parameters (p. )

Variation

Rate

Default

sets the sizing function parameters to the default values, as determined by ANSYS Fluent based

Rate

Default

on the current mesh. After execution, the Default button becomes the Reset button.

Reset

resets the sizing function parameters to the prior values (that is, those displayed at the moment

the Default button was clicked). After execution, the Reset button becomes the Default button.

The Mesh Smoothing Parameters dialog box allows you to define the settings for the smoothing

method selected in the Smoothing tab of the Mesh Method Settings Dialog Box (p. ).

Controls

Spring Constant Factor

controls the spring stiffness.

Convergence Tolerance

controls the smoothing convergence.

specifies the maximum number of iterations that will be attempted.

Elements

controls the elements where spring-based smoothing is applied.

Tet in Tet Zones

(3D only) specifies that only cell zones with all tetrahedral elements get smoothed.

Tet in Mixed Zones

(3D only) specifies that tetrahedral elements in mixed element zones get smoothed.

Tri in Tri Zones

(2D only) specifies that only cell zones with all triangular elements get smoothed.

Tri in Mixed Zones

(2D only) specifies that triangular elements in mixed element zones get smoothed.

All

specifies that all element types get smoothed.

Laplace Node Relaxation

specifies how the update of the node positions is relaxed on boundaries where there is Laplacian

smoothing.

Verbosity

specifies whether to print smoothing residuals to the console. Setting this to  ensures that such residuals

Verbosity

are printed, whereas the default value of  suppresses such output.

Diffusion Function

specifies whether the diffusion coefficient is a function of the Boundary Distance (Equation . (p. ))

or the Cell Volume (Equation . (p. )).This drop-down list is only available for diffusion-based

Diffusion Parameter

specifies  in Equation . (p. ) or Equation . (p. ), depending on the selected Diffusion Function.

This number-entry box is only available for diffusion-based smoothing.

AMG Stabilization

selects the algebraic multigrid (AMG) stabilization method used by the linear solver to perform mesh

smoothing calculations.This drop-down list is only available for smoothing based on diffusion (when

using the finite element method) or the linearly elastic solid model.

Relative Convergence Tolerance

specifies the relative residual tolerance for smoothing based on diffusion or the linearly elastic solid

model.

Generalized Boundary Distance Method

is an option that is available when you have selected Boundary Distance for the Diffusion Function,

and it allows you to use of a “generalized” boundary distance for the diffusion coefficient calculation.

When this option is enabled, the calculation uses the normalized distance to the nearest boundary that

is not declared as deforming, regardless of type; when it is disabled, only wall boundaries are considered.

Smoothing From Reference Position

enables smoothing from a reference position. Such smoothing may produce greater mesh quality consist-

ency for stationary or moving meshes with periodic or quasi-periodic motion. It is available when the

smoothing method is based on diffusion or the linearly elastic solid model; it is not available with layering,

remeshing, and/or dynamic adaption.

Poisson’s Ratio

specifies the linearly elastic solid material property  in Equation . (p. ).This number-entry box is

only available for smoothing based on the linearly elastic solid model.

The Mesh Scale Info dialog box allows you to inspect the values of minimum and maximum length

scale and maximum cell/face skewness in a mesh.

Controls

displays the minimum length scale in the mesh.

displays the maximum length scale in the mesh.

displays the maximum cell skewness in the zone.

displays the maximum cell skewness in the surface mesh.

The Options dialog box allows you to set the parameters for the options available in the Options

group box of the Dynamic Mesh task page.

Controls

contains parameters to be specified for the in-cylinder model. See In-Cylinder Settings (p. ) for more

Crank Shaft Speed

specifies the speed of the crank shaft.

Starting Crank Angle

specifies the starting crank angle.

Crank Period

specifies the crank period.

Crank Angle Step Size

specifies the crank angle step size used to determine the time step size to advance the solution.

Crank Radius

specifies the crank radius to calculate the piston location.

Piston Pin Offset

specifies the perpendicular offset of the piston pin from the plane defined by the crank shaft axis and

the direction of motion of the piston.The sign of this value is positive if top-dead-center (TDC) occurs

prior to a crank angle of °.

Connecting Rod Length

specifies the length of the connecting rod.

Piston Stroke Cutoff

specifies the piston stroke cutoff used to control the onset of layering in the cylinder chamber.

Minimum Valve Lift

specifies the minimum valve lift.

Write In-Cylinder Output

enables or disables the writing of in-cylinder specific output parameters.When this option is enabled,

the Output Controls... button becomes active.

Output Controls...

displays the In-Cylinder Output Controls Dialog Box (p. ) and is available only after the Write In-

Cylinder Output option is enabled.

Six DOF

contains parameters to be specified for the six degrees of freedom (DOF) solver. See Six DOF Solver Set-

tings (p. ) for more information.

Six DOF Properties

displays a list of defined sets of six DOF properties.

opens the Six DOF Properties Dialog Box (p. ).

Delete

removes the selected set of six DOF properties from the Six DOF Properties list.

Delete All

removes all sets of six DOF properties from the Six DOF Properties list.

contains the text entry boxes for gravitational acceleration in X,Y, and Z directions.

X,Y, Z

specifies the gravitational acceleration in X,Y, and Z directions respectively.

Write Motion History

allows you to keep track of an object’s motion history.

File Name

allows you to specify a file name for saving the object’s motion history.

File Name

contains parameters to be specified for implicit mesh updating. See Implicit Update Settings (p. ) for

Update Interval

allows you to specify the frequency in iterations at which the mesh will be updated within a time

step.

Motion Relaxation

allows you to set a value (within the range of  to ) for

in Equation . (p. ), which defines

the relaxation of the motion (that is, displacement of the nodes) during the mesh update.

Residual Criteria

allows you to set the relative residual threshold that is used to check the motion convergence.

contains parameters to be specified for contact detection. See Contact Detection Settings (p. ) for more

Face Zones

allows you to select the face zones that will be involved in contact detection.

Proximity Threshold

allows you to set the threshold below which the user-defined function for contact detection will be

invoked.

UDF

allows you to specify the user-defined function that will be invoked when contact has been detected.

Flow Control

allows you to indicate whether flow control zones are going to be used in the contact detection

process.

Controls...

opens the Flow Controls Dialog Box (p. ) where you can make additional flow control settings.

The In-Cylinder Output Controls dialog box contains parameters that control the output for the in-

cylinder model. See In-Cylinder Settings (p. ) for more information.

Controls

Controls

represents an integer entry specifying the interval in number of time-steps. Make sure that a value other

than  is used for the frequency, in order to allow you to complete your setup.

contains a drop-down list that allows you to select the method to calculate the swirl center.The list contains

calculates the swirl center inside the code and is used as the center of gravity of the chosen cell zones.

fixed

enables you to specify a swirl center in the X, Y, and Z entry fields below the drop-down list.

In addition to these two options, you can chose to use your own Compiled user-defined function

to calculate the swirl center. For details on using a dynamic mesh UDF, see the separate Fluent

Cell Zones

Swirl Axis

specifies the swirl axis with three entries for the directional components. By default, X, Y, Z= , , .

File Name

File Name

The Six DOF Properties dialog box allows you to define a set of properties for a rigid body dynamic

object that uses the Six DOF solver. The set of properties that you create can then be selected in the

Six DOF UDF/Properties drop-down in the Dynamic Mesh Zones Dialog Box (p. ) for the zones that

make up the object. See Setting Rigid Body Motion Attributes for the Six DOF Solver (p. ) and Rigid

Body Motion (p. ) for more information.

Controls

Name

specifies the name of the set of properties, which will be selectable in the Six DOF UDF/Properties drop-

down in the Dynamic Mesh Zones Dialog Box (p. ).

Mass

defines the mass of the rigid body dynamic object.

One DOF Translation

specifies that the dynamic object will only undergo one DOF translation.

One DOF Rotation

specifies that the dynamic object will only undergo one DOF rotation.

One DOF

contains settings that define the one DOF translation or rotation.

Direction

defines the vector along which the object will be allowed to translate.

Axis

defines the components of the axis of rotation. Note that for 2D cases, the axis will be either the

positive or negative z direction, depending on the sign of the value you enter for Z.

Center of Rotation

defines the point about which the object rotates.

Spring

contains settings that define an optional Hooke's law spring that can exert forces / torques on the

object. It is a compression / extension spring for translations, and it is a torsion spring for rotations.

Preload

Preload

defines a spring load that is constantly applied to the object, in addition to the loading resulting

from the spring Constant.The Preload can be a positive or negative value, and is defined relative

to the Direction (for translation) or the Axis (for rotation).

Constant

defines the spring constant / rate.

Constrained

specifies that the range of motion of the object is limited, as defined by the settings in the Reference

Point group box (for translation) or the Reference Angle group box (for rotation).

Reference Point

contains settings that define the limits of the object's translation when the Constrained option is

enabled.

Location

assigns a coordinate value to a point located on the object in its initial position; the Minimum

and Maximum coordinates are then defined relative to this value along the Direction vector, in

order to establish the limits of translation.

Minimum

defines the lower extent of the constrained translation along the Direction vector, relative to the

Location.

Maximum

defines the upper extent of the constrained translation along the Direction vector, relative to

the Location.

Reference Angle

contains settings that define the limits of the object's rotation when the Constrained option is enabled.

Value

assigns an angular coordinate value to the orientation of the object in its initial position; the

Minimum and Maximum angles are then defined relative to this orientation about the axis of

rotation, in order to establish the limits of rotation.

Minimum

defines the lower extent of the constrained rotation about the axis of rotation, relative to the

Value.

Maximum

Minimum

Value.

Maximum

defines the upper extent of the constrained rotation about the axis of rotation, relative to the

Value.

Moment of Inertia

defines the moment of inertia for the rigid body dynamic object that undergoes one degree of freedom

(DOF) rotation.

Inertia Tensor

defines the components of the inertia tensor for the object during six DOF motion. Note that the values

are relative to the Center of Gravity and Rigid Body Orientation settings defined in the Dynamic Mesh

Zones Dialog Box (p. ); the latter settings allow you to use a coordinate system that is local (rather than

global), if that is more convenient.

The Flow Controls dialog box allows you to specify flow control cell zones that are going to be used

in the contact detection process. See Contact Detection Settings (p. ) for more information.

Controls

Cell Zones

is a list that displays the names of all existing cell zones.

Settings

contains flow control zone settings.

Flow Control Zone

allows you to specify a name for the flow control zone.

Create Zone

allows you to create a new flow control zone of the specified name.

Delete Zone

allows you to delete the selected flow zone.

The Dynamic Mesh Events dialog box is available to control the timing of specific events during the

course of the simulation. See Defining Dynamic Mesh Events (p. ) for details.

Controls

Number of Events

specifies the number of events to be defined.

On

enables the corresponding event.

Name

specifies the name of the event.

At Crank Angle

Controls

On

Name

specifies the angular location of the crank at which the event should occur.This option appears for in-

cylinder flows.

At Time

specifies the time (in seconds) at which you want the event to occur.This option appears for non-in-cyl-

inder flows.

Define...

opens the Define Event Dialog Box (p. ).

Read...

opens The Select File Dialog Box (p. ).

Write...

Preview...

opens the Events Preview Dialog Box (p. ).

The Define Event dialog box allows you to define events.

Controls

Name

contains the name of the event to be defined.

Type

specifies the type of event.You can choose the type of event from the drop-down list.These event types

and their definitions are described in Events (p. ).

contains the input parameters corresponding to the type of event selected under Type.

Zone

contains a selectable list of the zones.The selection specifies the name of the zone(s) to be changed.

This item will appear only for the Change Zone Type event.

New Zone Type

specifies the type of zone to which an existing zone must be changed.This item will appear only for

the Change Zone Type event.

From Zone

specifies the name of the zone from which the boundary condition is to be copied.This item will appear

only for the Copy Zone BC event.

To Zone(s)

specifies the name of the zone to which the boundary condition is to be copied.This item will appear

Zone(s)

To Zone(s)

Zone(s)

contains a selectable list of the zones.The selection specifies the name of the zone to be activated/de-

activated.This item will appear only for the Activate Cell Zone and Deactivate Cell Zone events.

Interface Name

contains the name of the interface to be created or deleted.This item will appear only for the Create

Sliding Interface and Delete Sliding Interface events.

Interface Zone , Interface Zone

specifies the two zones on either side of the interface to be created.This item will appear only for the

Create Sliding Interface event.

Wall  Motion,Wall  Motion

specifies the dynamic zones whose motion can be copied for the zones specified under Interface

Zone  and Interface Zone .This item will appear only for the Create Sliding Interface event.

Attribute

allows you to select the relevant motion attribute.This item will appear only for the Change Motion

Attribute event.

Status

allows you to enable or disable the motion attribute.This item will appear only for the Change Motion

contains a list of dynamic zones.This item will appear only for the Change Motion Attribute event.

specifies the new physical time step value in degrees.This item will appear only for the Change Time

Step Size event.

Base Dynamic Zone

specifies the zone from which the layer of cells is to be created.This item will appear only for the Insert

Boundary Layer and Remove Boundary Layer event.

Side Dynamic Zone

This item will appear only for the Insert Boundary Layer event.

Internal Zone  Name, Internal Zone  Name

specifies the name of the new internal zones.

Time Step Size

allows you to change the time step size of the event.This item will appear only for the Change Time

allows you to specify the under-relaxation factors for the selected event.This item will appear only

for the Change Under-Relaxation Factors event. See Setting Under-Relaxation Factors (p. ) for

details.

Adjacent Dynamic Face Zone

allows you to select the dynamic face zone adjacent to the location of the cell layer to be inserted (or

deleted).You can select the required zone from the drop-down list.

Direction Parameter

is the direction with respect to the selected dynamic face zone a layer of cells is removed or added.

Command

specifies the series of text / Scheme commands or the macro to be executed during the simulation.

This item will appear only for the Execute Command event.

The Events Preview dialog box allows you to play the events to check that they are defined correctly.

Controls

specifies the crank angle at which you want to start the preview (for in-cylinder flows).

Start Time

specifies the time at which you want to start the preview (for non-in-cylinder flows).

End Crank Angle

specifies the crank angle at which you want to end the preview (for in-cylinder flows).

End Time

specifies the time at which you want to end the preview (for non-in-cylinder flows).

Increment

End Time

Increment

specifies the size of the step to take during the preview.

Preview

plays back the events at the crank angle specified for each event and reports when each event occurs in

the text (console) window.

The Dynamic Mesh Zones dialog box allows you to specify the motion of the dynamic zones in your

model. See Specifying the Motion of Dynamic Zones (p. ) for details.

Controls

Zone Names

contains the names of the zones in the model.

Type

contains the types of motion that can be specified for a dynamic zone.

Stationary

explicitly declares the zone as stationary, so that the nodes on this zone are excluded when updating

the node positions. See Specifying the Motion of Dynamic Zones (p. ) for more information.

Rigid Body

specifies the zone as having a rigid-body motion.

Deforming

specifies the zone as deforming.

enables you to specify a user-defined zone motion.

System Coupling

allows the zone to be involved in a system coupling simulation where the motion is defined by the

application that ANSYS Fluent is coupled with on this zone (see the Fluent in Workbench User's Guide

and the System Coupling Guide for more details). Once enabled, the Solver Options tab can be used

to help achieve convergence for system coupling cases where the physics is strongly coupled. If a

dynamic mesh zone of the type System Coupling exists, and ANSYS Fluent is not involved in a system

Intrinsic FSI

specifies that a wall zone between a fluid and solid cell zone deforms according to the deformation

of the adjacent solid zone as part of a two-way intrinsic fluid-structure interaction (FSI) simulation.

Note that this type can only be used for the side of a two-sided wall (that is, the wall or wall-shadow)

that is immediately adjacent to the fluid cell zone (as indicated by the Adjacent Cell Zone field in

the Wall dialog box).This option is only available when a model is selected in the Structural Model

lists all of the dynamic zones in the case.

Motion Attributes

contains parameters to specify the motion attributes for a rigid-body-motion zone and a user-defined-

motion zone.

Motion/UDF Profile

allows you to define the motion of the rigid body zone by selecting a profile or user-defined function

from the drop-down list. See Profiles (p. ) and Solid-Body Kinematics (p. ) for information on

profiles, and see the Fluent Customization Manual for information on user-defined functions.

Six DOF UDF/Properties

allows you to define the motion of a rigid body zone by selecting a profile, user-defined function, or

set of six DOF properties (created using the Six DOF Properties Dialog Box (p. )) from the drop-

down list.This option is available only when On is enabled in the Six DOF group box.

Six DOF

contains parameters for the Six DOF solver.

On

enables the use of the Six DOF solver.

Passive

(if enabled) does not take forces and moments on the zone into consideration.

Center of Gravity Location

specifies the initial values of the coordinates for the location of the center of gravity of the selected

zone.This item will appear only if the motion Type is Rigid Body and In-Cylinder is not enabled in

the Dynamic Mesh task page. After calculating, ANSYS Fluent updates these fields, allowing you to

keep track of the object's current location.

Motion Options

provides a Relative Motion option, which allows you to specify that the motion of the dynamic zone

is relative to another pre-defined rigid body zone.This group box will only appear if the Type is Rigid

Body or User-Defined; for the latter, the Relative Zone must be a cell zone.

Rigid Body Orientation

specifies the initial values that define the orientation of the rigid body of the selected zone.This item

will appear only if the motion Type is Rigid Body and In-Cylinder is not enabled in the Dynamic

Mesh task page. After calculating, ANSYS Fluent updates these fields, allowing you to keep track of

the object's current orientation.

Center of Gravity Velocity

specifies the velocity of the center of gravity with respect to inertia coordinate system.This option is

available only if the Six DOF solver is the selected model.

Rigid Body Angular Velocity

specifies the angular velocity of the rigid body with respect to inertia coordinate system.This option

is available only if the Six DOF solver is the selected model.

Lift/Stroke

contains the current value of valve lift or piston stroke, which is automatically updated when you

click Create.This item will appear only if In-Cylinder is enabled in the Dynamic Mesh task page.

Valve/Position Axis

specifies the direction of the reference axis of the valves or piston for an in-cylinder problem.This

item will appear only if In-Cylinder is enabled in the Dynamic Mesh task page.

Mesh Motion UDF

allows you to select the user-defined function that defines the geometry and motion of the zone.

This item will appear only if the motion Type is User-Defined.

Exclude Mesh Motion in Boundary Conditions

allows you to specify that the boundary mesh motion should not be included in the physical boundary

conditions of that zone.This option is only available for non-periodic boundary zones.

Geometry Definition

contains parameters to define a deforming zone.

allows you to select a geometry definition to project nodes of the deforming zone on. Available options

are faceted, plane, cylinder, and user-defined.

Feature Options

allows you to preserve features for 3D cases on boundary zones of type Deforming or User-Defined.

Such features may be at the juncture of different boundary zones, or they may be on a single non-

planar boundary zone.

Feature Detection

enables the detection and preservation of features of a particular angular range.

defines a threshold value in degrees. For details on how this angle is defined, see Feature Detec-

tion (p. ).

Point on Plane

allows you to specify the position of a point on the plane.This item will appear only when you select

plane for the Definition.

Plane Normal

allows you to specify the direction of the plane normal.This item will appear only when you select

Cylinder Radius

allows you to specify the radius of the cylinder.This item will appear only when you select cylinder

for the Definition.

Cylinder Origin

allows you to specify the location of the cylinder origin.This item will appear only when you select

cylinder for the Definition.

Cylinder Axis

allows you to specify the direction of the cylinder axis.This item will appear only when you select

Geometry UDF

allows you to select a user-defined function for a geometry Definition.

Meshing Options

contains parameters for various meshing options.

Adjacent Zone

contains the name of the adjacent zone that is involved in local remeshing or dynamic layering.This

item will appear only if the zone type is Stationary, Rigid Body, User-Defined, or Intrinsic FSI, and

if the zone is not the boundary of a CutCell dynamic cell zone.

Cell Height

allows you to specify the ideal height of the adjacent cells as either a constant value or a compiled

user-defined function.This item will appear only if the motion Type is Stationary, Rigid Body, User-

Defined, or Intrinsic FSI, and if the zone is not the boundary of a CutCell dynamic cell zone.

Deform Adjacent Boundary Layer with Zone

enables the smoothing of an adjacent boundary layer mesh.This option is not available when Sta-

tionary or Deforming is selected in the Type list.

Remeshing

enables remeshing for a deforming zone, and allows you to use the settings in the group box below

to specify whether the global settings defined in the Remeshing tab of the Mesh Method Settings

Dialog Box (p. ) are applied to this zone.The settings that are available in the group box are based

on whether you are defining a boundary zone or a cell zone, and on the global remeshing settings.

provides remeshing settings for boundary zones or cell zones that are not CutCell zones.

Global Settings

allows you to specify that this deforming zone uses the settings you defined globally in the

Remeshing tab of the Mesh Method Settings dialog box.When this option is disabled, you

can use the other settings under Parameters to define unique local remeshing criteria.

specifies the lower limit of cell size below which the cells are marked for remeshing for the

zone.

specifies the upper limit of cell size above which the cells are marked for remeshing for the

zone.

Maximum Skewness

specifies the desired value for maximum skewness in the zone.

Zone Scale Info...

opens the Zone Scale Info Dialog Box (p. ), in which you can view the statistics of the zone,

such as minimum, maximum, and average length scale values, as well as the maximum

skewness.

Options

provides remeshing options for the zone.

Region

enables the region-based remeshing method for boundary zones.

Local

enables the local face remeshing method for boundary zones.

CutCell

enables the CutCell zone remeshing method for cell zones.

CutCell Zone Parameters

provides a set of global parameters used for CutCell zone remeshing.These settings will only

appear if the CutCell option is enabled under Options.

Maximum Mesh Size

specifies the maximum mesh size of the Cartesian CutCell mesh.

specifies the default growth rate used for mesh refinement by size functions.This growth rate

is used during remeshing by the mesh-based size functions of all boundaries of the CutCell

cell zone that are not defined as dynamic mesh zones.

Minimum Orthogonal Quality

specifies the minimum allowable orthogonal quality for the cell zone. CutCell remeshing will

occur if the orthogonal quality for any cell in the cell zone drops below this value.

Remeshing Interval

specifies the interval of time steps at which the cell zone remeshing will take place, even if

the mesh quality has not deteriorated below the value entered for Minimum Orthogonal

Quality. Enter a value of  for the Remeshing Interval if you want the remeshing to occur

only if there is insufficient mesh quality.

Inflation Layers

allows you to enable inflation layers on the CutCell cell zone and specify global inflation

opens the Inflation Settings Dialog Box (p. ), which allows you to enter the global inflation

parameters used by default on all boundary zones.

opens the Zone Scale Info Dialog Box (p. ), in which you can view the statistics of the mesh,

skewness.

Boundary Zones Info...

opens the CutCell Boundary Zones Info Dialog Box (p. ), which lists all of the boundary

zones for the CutCell dynamic cell zone, along with the remeshing and inflation layer para-

meters.

CutCell Boundary Zone Parameters

meters.

provides a set of local parameters used for CutCell zone remeshing.This group box will only appear

if the zone is a boundary of a CutCell dynamic cell zone.

specifies the maximum mesh size used by the soft size function. If a value of  is entered, a

mesh-based size function is used to locally refine the Cartesian mesh near the boundary.

specifies the local growth rate used by the size function.

Zonal Inflation Layer Control

allows you to enable local inflation layer control and specify local inflation parameters.This

option is only available if Inflation Layers has been enabled for the CutCell dynamic cell zone.

If Zonal Inflation Layer Control is not enabled, then the global inflation parameters specified

for the cell zone are used.

opens the Inflation Settings Dialog Box (p. ), which allows you to enter local inflation

parameters for the CutCell boundary zone.

skewness.

Smoothing

enables smoothing for a deforming zone, and allows you to use the settings in the group box below

to specify whether the global settings defined in the Smoothing tab of the Mesh Method Settings

Dialog Box (p. ) dialog box and the Mesh Smoothing Parameters Dialog Box (p. ) are applied to

this zone.The settings that are available in the group box are based on whether you are defining a

boundary zone or a cell zone, and on the global smoothing settings.

Elements

Elements

allows you to specify the element types for which spring-based smoothing is used in this zone.

This will only be available if you are defining a cell zone and the Spring/Laplace/Boundary

Layer method has been selected in the Smoothing tab of the Mesh Method Settings dialog

box.

allows you to specify that this deforming zone smooths the element types you specified

globally in the Mesh Smoothing Parameters Dialog Box (p. ).When this option is disabled,

you can make a unique local selection using the radio buttons below.

(3D only) specifies that this zone will get smoothed only if it consists entirely of tetrahedral

elements.

(3D only) specifies that all tetrahedral elements in this zone should get smoothed. All other

elements in a mixed element zone will not undergo smoothing.

(2D only) specifies that this zone will get smoothed only if it consists entirely of triangular

elements.

(2D only) specifies that all triangular elements in this zone should get smoothed. All other

All

specifies that all element types in this zone will get smoothed.

Methods

allows you to specify the smoothing method for the zone.This is only available if you are defining

a boundary zone and the Spring/Laplace/Boundary Layer method has been selected in the

Smoothing tab of the Mesh Method Settings dialog box.

Spring

enables the spring-based smoothing method for this zone.

Laplace

Spring

Laplace

enables the Laplacian smoothing method for this zone.

Remeshing Method

provides settings for local face remeshing of the dynamic zone.This group box will appear only for

boundary zones, when the motion Type is User-Defined.

Local

enables local face remeshing for the dynamic zone.This option is only available when Local Face

is enabled in the Remeshing tab of the Mesh Method Settings Dialog Box (p. ).

is a field that, if revised (with a reasonable value), sets a maximum skewness for the local face

remeshing of the dynamic zone that is different than the global value set in the Remeshing tab

of the Mesh Method Settings Dialog Box (p. ).

Solver Options

contains settings that may help convergence for boundary zones in cases that involve strong fluid-

structure interaction (notably zones undergoing rigid body motion with the six degrees of freedom

solver, system coupling motion, or two-way intrinsic FSI motion). See Solution Stabilization for Dynamic

Mesh Boundary Zones (p. ) for more information.

Solution Stabilization

enables/disables solution stabilization settings for boundary zones.

Stabilization Parameters

contains options for solution stabilization settings.

Scale Factor

allows you to set the scale factor used by the selected Method for convergence stabilization.

Method

Stabilization is achieved through a boundary source coefficient introduced in the continuity

equation. It is designed to improve the diagonal dominance of the matrix system in the cells ad-

jacent to the boundary zone.Two methods for this boundary source coefficient are available:

specifies that the diagonal entry of the linear matrix system corresponding to the discretized

continuity equation is re-scaled using the cell volume and a scale factor, according to Equa-

(default) specifies that the diagonal entry of the linear matrix system corresponding to the

discretized continuity equation is directly re-scaled by a scale factor, according to Equa-

The Orientation Calculator dialog box allows you to convert rotation matrices and Euler angles to

axis and angle format. It also allows you to concatenate rotations to determine a rigid body’s final

orientation.

Controls

Input Type

allows you to select which method you will use to enter your rigid body orientation values. For additional

information about these input types, see Rigid Body Motion (p. ).

Axis and Angle

allows you to enter the angle of rotation and the axis about which the rigid body is rotating.

Rotation Matrix

allows you to enter the orientation of the rigid body as a rotation matrix.

Euler Angles

allows you to enter the orientation of the rigid body as a set of Euler Angles. For an explanation of which

Euler angles method Fluent uses, see Rigid Body Motion (p. ).

Output

displays the angle of rotation and the axis about which the rigid body is rotating after you click Evaluate.

Note that if you enter a single orientation in Axis and Angle and click Evaluate, the values shown

in Output will be the same as you entered in Axis and Angle

Concatenate Next Input

concatenates the next input entered (after clicking Evaluate) to the values displayed in Output

Evaluate

converts the specified input values into angle and axis format and displays the results in Output.

Note that the calculator also converts the entered values into the other two “grayed-out” input formats.

Fill

enters the values displayed in Output into the Rigid Body Orientation field of the Dynamic Mesh Zones

The Inflation Settings dialog box allows you to enter inflation layer parameters for a dynamic zone.

Controls

Offset Method

allows you to select how the first layer height is evaluated.The constant type will use the same first

height for all elements.The aspect-ratio type will evaluate local first heights such that the aspect ratio

(base size divided by the element height) of the resulting elements is constant.

First Aspect Ratio

allows you to specify the aspect ratio of the first element if the Offset Method is set to aspect-ratio.

First Height

allows you to specify the height of the first element if the Offset Method is set to constant.

allows you to specify the geometric growth rate of the inflation element heights.

Number of Layers

allows you to specify the number of elements in the inflation layer.

Last Aspect Ratio

displays the aspect ratio of the last element for the given set of parameters if the Offset Method is set

to aspect-ratio.

displays the overall thickness of the inflation layer if the Offset Method is set to constant.

The CutCell Boundary Zones Info dialog box displays a list of all of the boundary zones for the CutCell

dynamic cell zone. This list also provides the remeshing parameters for the zones, including size

function type, the maximum mesh size, the growth rate used to refine the mesh at all of the CutCell

boundaries. The inflation layer settings used on all boundaries are also shown.

The Zone Scale Info dialog box allows you to inspect the values of minimum and maximum cell area

or volume, and maximum cell skewness in a zone.

Controls

displays the maximum cell length in the zone.

displays the minimum cell length in the zone.

Average Length Scale

displays the average cell length in the zone.

The Zone Motion dialog box will display the motion of zones specified with Rigid Body or User-

Defined motion. See Previewing the Dynamic Mesh (p. ) for details about the items below.

Controls

Time Control

contains controls to specify the time intervals at which to display the motion.

Start Time (s)

specifies the time from which to start the zone motion preview.

Time Step (s)

specifies time step size for zone motion preview.

Number of Steps

specifies number of time steps for zone motion preview.

Dynamic Face Zones

allows you to select the dynamic face zones to preview. Only User-Defined or Rigid Body zones are

Preview

previews the zone motion.

Reset

Preview

Reset

resets the zone display and the dialog box inputs.

The Mesh Motion dialog box allows you to preview the dynamic mesh as it changes with time before

you start your simulation. See Previewing the Dynamic Mesh (p. ) for details.

Controls

Time

contains the parameters to specify the time interval at which to update the mesh.

Current Mesh Time

displays the current time after the dynamic mesh has been advanced the specified number of steps.

specifies the size of each time step.

specifies the number of time steps.

Options

contains options to view the updated mesh.

Display Mesh

displays the mesh.

opens the Save Picture Dialog Box (p. ), allowing you to save a picture file of the mesh each time

ANSYS Fluent updates it during the mesh preview.

Enable Autosave

opens the Autosave Case During Mesh Motion Preview Dialog Box (p. ), allowing you to save the

case and data files with the specified name and frequency. See Automatic Saving of Case and Data

Files (p. ) for details.

Update Mesh Interfaces

allows you to update the interface at every time step.

Update Monitors

allows you to disable the processing of monitors and computation activities during mesh motion

preview.

Display Frequency

displays the frequency at which ANSYS Fluent will update the mesh display.

Preview

allows you to preview the motion of the selected zones in the graphics window.

Preview

The Autosave Case During Mesh Motion Preview dialog box allows you to automatically save your

case during the dynamic mesh preview as it changes with time, while running your simulation. See

Automatic Saving of Case and Data Files (p. ) for details about the inputs.

Controls

Save Case File Every

Retain Only the Most Recent Files

allows you to restrict the number of files saved by ANSYS Fluent if you have limited disk space.When this

option is enabled, you can enter the appropriate value in the Maximum Number of Data Files field.

Note

Only the associated case files are retained when using this option.

Maximum Number of Data Files

specifies the maximum number of data files that can be saved at any instance. If you have constraints on

the disk space, you can restrict the number of files to be saved using this field. After saving the specified

number of files, ANSYS Fluent will overwrite the earliest existing file.The default value for this field is zero,

which saves all the files.

Append File Name with

allows you to select flow-time or time-step to be appended to the file name.This option is available

only for unsteady-state calculations.The default selection is flow-time.

The Reference Values task page allows you to set the reference quantities used for computing normal-

ized flow field variables. It also allows you to specify the reference zone for postprocessing relative ve-

locities in moving-zone problems. See Reference Values (p. ) for details about the items below.

Controls

Compute from

contains a drop-down list of the boundary zones.You may select a zone to be used for automatically de-

fining the reference values, but depending on the boundary condition used, all of the reference values

may not be set. For example, the reference length and area will not be set by computing the reference

values from a boundary condition; you must set these manually.

contains inputs for the reference values.

Area

sets the reference area, which is used to compute the force and moment coefficients.

Depth

sets the reference depth used for computing cell volumes in 2D.

Reference Values Task Page

Density

sets the reference density, which is used to compute the reference dynamic pressure.

Enthalpy

sets the reference enthalpy, which is used to determine the total enthalpy change.

Length

sets the reference length, which is used in the computation of the moment coefficient.

Pressure

sets the reference pressure, which is used to compute the pressure-related forces and moments and

the pressure coefficient.

sets the reference temperature, which is used to compute entropy for incompressible flows.

Velocity

sets the reference velocity magnitude, which is used to compute the reference dynamic pressure.

Viscosity

sets the reference kinematic viscosity, which is used in the computation of the boundary Reynolds

number.

Ratio of Specific Heats

sets the value of the specific heat ratio, which is used in turbomachinery efficiency calculations.

Reference Zone

number.

contains a drop-down list of all cell zones in the domain. For flows involving multiple moving zones, you

must select the reference zone for postprocessing relative velocities and related quantities. See Setting

the Reference Zone (p. ) for details.

The Solution task page introduces you to the main tasks involved in solving your CFD simulation using

ANSYS Fluent. For more information about using ANSYS Fluent to solve your CFD simulation, see Using

the Solver (p. ).

The Solution Methods task page allows you to specify various parameters associated with the solution

method to be used in the calculation.

Controls

provides a drop-down list of the available types of solver formulations: Implicit and Explicit.

This item appears only when the density-based solver is used.

Flux Type

provides a drop-down list of the convective flux types: Roe-FDS, AUSM, and Low Diffusion Roe-FDS.

Details about each of the flux types can be found in Convective Fluxes in the Theory Guide.

contains settings for pressure-velocity coupling schemes.

Scheme

(for the pressure-based solver only) provides a drop-down list of the available pressure-velocity coupling

schemes: SIMPLE, SIMPLEC, PISO, and Coupled.When the non-iterative time advancement (NITA)

scheme is enabled in the Solution Methods task page, Fractional Step is available for single phase

Solution Methods Task Page

flows, and Phase Coupled SIMPLE is available for Eulerian multiphase flows. See Pressure-Velocity

Coupling in the Fluent Theory Guide, and Choosing the Pressure-Velocity Coupling Method (p. ),

Setting Solution Controls for the Non-Iterative Solver (p. ), and Selecting the Pressure-Velocity

Coupling Method (p. ) for details about these methods.

Skewness Correction

enables the SIMPLEC and PISO skewness correction for highly skewed meshes if the value (number of

iterations) is greater than .The default value is  for SIMPLEC and  for PISO.

Neighbor Correction

enables the PISO neighbor correction, which is recommended for transient calculations, if the value

(number of iterations) is greater than .The default value is .

Skewness-Neighbor Coupling

allows for a more economical but a less robust variation of the PISO algorithm.

Coupled with Volume Fraction

couples velocity corrections, shared pressure corrections, and the correction for volume fraction sim-

ultaneously.This option is available in the interface after you have selected Coupled from the Scheme

drop-down list for Pressure-Velocity Coupling.

Solve N-Phase Volume Fraction Equations

solves all primary and secondary volume fraction equations and scales the resulting volume fractions

to satisfy the requirement that they sum to . If this is disabled, only the secondary phase volume

fractions are solved directly and the primary phase volume fraction is set such that the volume fractions

sum to .

contains settings that control the spatial discretization of the convection terms in the solution equations.

See Choosing the Spatial Discretization Scheme (p. ) for details.

Gradient

Gradient

contains a drop-down list of the options for setting the method of computing the gradient in Equa-

tion . in the Theory Guide: Green-Gauss Cell Based; Green-Gauss Node-Based, and Least Squares

Cell Based. See Evaluation of Gradients and Derivatives in the Theory Guide for details.

Pressure

(for the pressure-based solver only) contains a drop-down list of the discretization schemes available

for the pressure equation: Standard, PRESTO!, Linear, Second Order, and Body Force Weighted.

This item appears only when the pressure-based solver is used.

Flow

(for the density-based solvers only) contains a drop-down list of the discretization schemes available

for the pressure, momentum, and (if relevant) energy equations: First Order Upwind, Second Order

Upwind, Third-Order MUSCL, and (if the LES, DES, SAS, SDES, or SBES turbulence model is enabled)

Bounded Central Differencing.

This item appears only when one of the density-based solvers is used.

Momentum, Energy, and so on

are the names of the other convection-diffusion equations being solved. In the drop-down list next to

each equation, you can select the First Order Upwind, Second Order Upwind, QUICK, or Third-Order

MUSCL discretization scheme for that equation.

If the LES, DES, SAS, SDES, or SBES turbulence model is enabled, then you have a choice of se-

lecting Bounded Central Differencing or Central Differencing for Momentum.

If one of the density-based solvers is used, Momentum and Energy will not appear. For the

density-based solvers, the discretization scheme for these equations is selected in the Flow

drop-down list (described above).

is available when the VOF multiphase model is enabled.The discretization schemes that are used when

solving volume fraction equations for the VOF explicit scheme are Geo-Reconstruct, Compressive,

CICSAM, Modified HRIC, and QUICK.The discretization schemes that are used when solving volume

fraction equations for the VOF implicit scheme are First Order Upwind, Second Order Upwind,

Compressive, Modified HRIC, BGM (steady state only), and QUICK. See Interpolation Near the Interface

in the Theory Guide for detailed information about these VOF-specific interpolation schemes.

Transient Formulation

contains options for setting different time-dependent solution formulations.This option appears only

when Transient is enabled under Time in the General task page. Available options include: Explicit

(available only for the Density Based Explicit solver); First Order Implicit; Second Order Implicit; and

Bounded Second Order Implicit. See Performing Time-Dependent Calculations (p. ) for details.

Non-Iterative Time Advancement

enables non-iterative time-advancement (NITA) scheme. See Time-Advancement Algorithm in the Theory

Guide for details.

Accelerated Time Marching

enables a modified NITA scheme and other setting changes that can speed up the simulation.This option

is only available with the Large Eddy Simulation (LES) turbulence model, and is intended for unreacting

flow simulations that use a constant-density fluid. For details, see Setting Solution Controls for the Non-

Iterative Solver (p. ).

Frozen Flux Formulation

enables an option to discretize the convective part of Equation . in the Theory Guide using the mass

flux at the cell faces from the previous time level n.This option is available only for a Transient solution.

See The Frozen Flux Formulation in the Theory Guide for details.

Pseudo Transient

enables an option to apply the pseudo transient under-relaxation method, which is a form of implicit under-

relaxation (see Pseudo Transient Under-Relaxation).This option is available for the pressure-based solver

when Coupled is selected as the Pressure-Velocity Coupling  scheme and for the density-based implicit

solver. Note that this method can only be used when running a steady-state simulation.

Warped-Face Gradient Correction

enables an adjustment to the gradient discretization method that improves the gradient accuracy for

meshes containing high aspect ratios, cells with non-flat faces, and highly deformed cells, and can help

avoid numerical difficulties in simulations that involve a mesh that has large differences in the volumes of

neighboring cells. By default, the fast, or more computationally efficient mode of the warped-face gradient

correction is used. For additional information about the warped-face gradient correction, see Warped-Face

Gradient Correction (p. ).

Convergence Acceleration For Stretched Meshes

Enable convergence acceleration for stretched meshes to improve the convergence of the implicit density

based solver on meshes with high cell stretching (see Convergence Acceleration for Stretched Meshes

(CASM) (p. )).

High Order Term Relaxation

enables the relaxation of high order terms to aid in the solution behavior of flow simulations when higher

order spatial discretization is used.

Opens the Relaxation Options Dialog Box (p. ).

Set All Species Discretizations Together

enables an option to use the same discretization scheme for all the species rather than setting each of the

species individually. Notice that you will no longer see your list of individual species, instead a Species

field will appear with the scheme of your choice. Note that this option is available when species transport

Default

sets the fields to their default values, as assigned by ANSYS Fluent.

Report Poor Quality Elements

reports statistics on the number and type of cells that ANSYS Fluent has identified as having poor quality.

... Relaxation Options Dialog Box

The Relaxation Options dialog box allows you to further control the High Order Term Relaxation

as described in High Order Term Relaxation (HOTR) (p. ).

Controls

Variables

allows you to select between under-relaxing All Variables or only the default flow variables (Flow Vari-

ables Only.

is by default . for steady-state cases and . for transient cases.

The Solution Controls task page allows you to set common solution parameters.

Controls

Controls

sets the fine-grid Courant number (time step factor) when the density-based solver is used. See Changing

the Courant Number (p. ) for guidelines on setting the Courant number.

When the pressure-based solver is used for time-independent flows, and the Coupled pressure-ve-

locity scheme is used, the Courant Number is used to stabilize the convergence behavior. See Under-

Relaxation of Equations in the Theory Guide for a correlation of the under-relaxation factor and

courant number.

Flow Courant Number

sets the Courant number for multiphase flow using the pressure-based coupled solver.The Flow Courant

Number is used to stabilize the convergence behavior.

Volume Fraction Courant Number

sets the Courant number for multiphase flow using the pressure-based solver is coupled with the volume

fraction.The default value is  and will appear in the interface when the Coupled with Volume Fraction

option appears in the Solution Methods task page.

Solution Controls Task Page

Explicit Relaxation Factors

for the Coupled scheme defines the explicit relaxation of variables between sub-iterations for momentum

and pressure. See Under-Relaxation of Variables in the Theory Guide for information.

Multigrid Levels

specifies the maximum number of coarse levels to be created by the FAS multigrid solver.This item is the

same as the Max Coarse Levels under FAS Multigrid Controls in the Multigrid tab of the Advanced

Solution Controls Dialog Box (p. ), and it appears only when the density-based explicit solver is used.

Residual Smoothing

contains parameters that govern the use of implicit residual smoothing. (See Implicit Residual Smoothing

in the Theory Guide and Using Residual Smoothing to Increase the Courant Number (p. ) for details.)

This section of the task page will appear only when the density-based explicit solver is used.

sets the number of iterations of the Jacobi smoother to use. If Iterations is , then no implicit residual

smoothing is performed.

Smoothing Factor

sets the implicit residual smoothing factor.This item will not appear unless Iterations is set to a non-

zero value.

contains the under-relaxation factors for all equations that are being solved with the pressure-based

solver. (See Setting Under-Relaxation Factors (p. ) for details.) In the field next to each equation, you

can set the under-relaxation factor for that equation.

When one of the density-based solvers is used, Under-Relaxation Factors will appear only for the

following variables, when they are included in your model: solid (for conjugate heat transfer models),

turbulence variables, and viscosity. The solid under-relaxation factor is used to scale the CFL value

in the solid region only if the under-relaxation value is set to a value less than . When the under-

relaxation value is set to , then the solver ignores the specified CFL value for the solid and instead

uses a very large value of CFL. This is done to speed up the convergence in the solid region. The

density-based solvers use a segregated method to solve these equations; all the other equations

are solved in a coupled manner, so there are no under-relaxation factors for them.

When Non-Iterative Time Advancement is selected for the pressure-based solver, the Non-Iterative

Solver Relaxation Factors define the explicit relaxation (Under-Relaxation of Variables in the Theory

Guide) of variables between sub-iterations and are used to prevent the solution from diverging.

When Pseudo Transient is selected (available with the pressure-based coupled solver), the Pseudo

Transient Explicit Relaxation Factors can be specified (see Setting Pseudo Transient Explicit Relax-

ation Factors (p. )).

Acoustics Wave Equation Solver Controls

contains parameters that govern the acoustics wave equation solver

Relative Convergence Criterion

sets the relative convergence criterion for the acoustics wave equation solver.

Max Itertation/Time Step

sets the maximum number of iterations per time step.

Default

displays the Equations Dialog Box (p. ).

Limits...

displays the Solution Limits Dialog Box (p. ).

displays the Advanced Solution Controls Dialog Box (p. ).

Set All Species URFs Together

enables an option to use the same under-relaxation factors for all the species rather than setting each of

the species individually. Notice that you will no longer see your list of individual species, instead a Species

field will appear with the specified under-relaxation factor. Note that this option is available when species

transport is enabled.

... Equations Dialog Box

... Solution Limits Dialog Box

... Advanced Solution Controls Dialog Box

The Equations dialog box contains a list of the equations being solved for the current model. To

temporarily disable solution of an equation, deselect it in this list and click OK. To re-enable the calcu-

lation for an equation, select it and click OK. See Step-by-Step Solution Processes (p. ) for details

about using this feature in a step-by-step solution process.

Note that, when one of the density-based solvers is used, Energy will not appear as a separate item

in the Equations list. For the density-based solvers the energy equation is included in the Flow category

(which also includes the pressure and momentum equations).

The Solution Limits dialog box allows you to improve the stability of the solution. See Setting Solution

Limits (p. ) for details about the items below.

Controls

Minimum Absolute Pressure, Maximum Absolute Pressure

set the limiting minimum and maximum allowable values for absolute pressure.

Minimum Static Temperature, Maximum Static Temperature

set the limiting minimum and maximum allowable values for temperature.

Minimum Turb. Kinetic Energy

sets the limiting minimum value of turbulent kinetic energy ( ) in the flow field.This parameter appears

when one of the -  or -

models or the RSM is used.

Minimum Turb. Dissipation Rate

sets the limiting minimum value of turbulent dissipation rate ( ) in the flow field.This parameter appears

when one of the -  models or the RSM is used.

Minimum Spec. Dissipation Rate

sets the limiting minimum value of specific dissipation rate (

) in the flow field.This parameter appears

when one of the -

models is used.

Maximum Turb.Viscosity Ratio

sets the limiting maximum allowable value of the ratio of turbulent to laminar viscosity (

).The tur-

bulent viscosity is reduced to the necessary value so as not to exceed the maximum allowable viscosity

ratio.

This parameter appears for all turbulent flows.

Minimum Vol. Frac. for Matrix Solution

sets the limiting minimum value for volume fraction in the matrix solution.This field appears for Eulerian

multiphase simulations run on a double-precision solver.

Positivity Rate Limit

sets the limiting value for the rate of reduction of temperature. See Adjusting the Positivity Rate Limit (p. )

Default

sets the fields to their default values, as assigned by ANSYS Fluent. After execution, the Default button

Reset

resets the fields to their most recently saved values (for example, the values before Default was selected).

After execution, the Reset button becomes the Default button.

The Advanced Solution Controls dialog box allows you to set parameters related to the multigrid,

multi-stage, and non-iterative solvers.

Controls

Multigrid

tab contains parameters related to the multigrid solver. See Modifying Algebraic Multigrid Paramet-

Controls

Multigrid

ers (p. ) and Setting FAS Multigrid Parameters (p. ) for details about the items below.

Cycle Type

contains a drop-down list for each equation that is being solved. From this list you can select the

multigrid cycle type (Flexible, V-Cycle, W-Cycle, or F-Cycle). See Specifying the Multigrid Cycle

Type (p. ) for details.

Note that, for the density-based solvers, the Pressure, Momentum, and Energy equations will

not appear individually. They will instead be grouped together and called Flow.

Furthermore, for the density-based explicit solver, the Cycle Type choices for the Flow equations

will be limited to V-Cycle and W-Cycle, while the choices for Flow for the density-based implicit

solver will be limited to V-Cycle and F-Cycle.

Termination

specifies the termination criterion for each equation that is being solved using algebraic multigrid.

See Setting the Termination and Residual Reduction Parameters (p. ) for details.

Restriction

specifies the residual reduction criterion for each equation that is being solved using the Flexible

algebraic multigrid cycle. See Setting the Termination and Residual Reduction Parameters (p. ) for

details. (This item will not appear for an equation that is using a V-Cycle, W-Cycle, or F-Cycle.)

Stabilization Method

contains the drop-down list to choose the stabilization method. For further details, see Setting the

Stabilization Method (p. ).

BCGSTAB

enables the bi-conjugate gradient stabilized method.

RPM

enables the recursive projection method. RPM stabilization is mainly used in conjunction with

BCGSTAB

RPM

the coupled pressure-based solver.

CG

enables the conjugate gradient method. CG stabilization is mainly used in conjunction with the

segregated pressure-based solver.

GMRES

enables the generalized minimal residual method. GMRES stabilization is recommended for cases

that fail to converge with the BCGSTAB method.

Algebraic Multigrid Controls

contains parameters related to the algebraic multigrid solver. See Algebraic Multigrid (AMG) in the

Theory Guide and Modifying Algebraic Multigrid Parameters (p. ) for details.

Scalar and Coupled Parameters

contain parameters that you can set, If you are using the density-based explicit solver or the

pressure-based solver with any of the segregated schemes, described in Pressure-Velocity Coupling

in the Theory Guide and Choosing the Pressure-Velocity Coupling Method (p. ), you will only

set Scalar Parameters. If you are using the density-based implicit or the pressure-based coupled

scheme, described in Coupled Algorithm, then you can set the Coupled Parameters.

Fixed Cycle Parameters

contains parameters that control the V,W, and F cycles.You can set the number of Pre-Sweeps

and Post-Sweeps, and the Max Cycles. Normally one post-sweep is performed and no pre-

sweeps are done. See Fixed Cycle Parameters (p. ) for details about using the items below.

Pre-Sweeps

sets the number of sweeps to perform before moving to a coarser level.

Post-Sweeps

sets the number of sweeps to perform after coarser level corrections have been applied.

Max Cycles

Max Cycles

sets the maximum number of V,W, or F cycles to be performed.The multigrid solver will

continue to solve the set of equations until either the maximum number of cycles has

been performed, or the Termination criteria are satisfied.

Coarsening Parameters

contains parameters that control the grouping of equations in the algebraic multigrid al-

gorithm. See Coarsening Parameters (p. ) for details

Max Coarse Levels

is the maximum number of coarse levels that will be built by the multigrid solver. Sets of

coarser simultaneous equations are built until the maximum number of levels has been

created, or the coarsest level has only  equations. Each level has about half as many un-

knowns as the previous level, so coarsening until there are only a few nodes left will require

about as much total coarse-level coefficient storage as was required on the fine mesh.

Reducing the maximum coarse levels will reduce the memory requirements, but may re-

quire more iterations to achieve a converged solution. Setting Max Coarse Levels to

turns off the multigrid solver.

Coarsen by

controls the number of equations on each successively coarser grid level. By default, this

parameter is set to , indicating that the number of equations on each level will be /

of the number on the previous level. In general, the number of equations on each coarser

grid level will be approximately equal to /  of the number on the previous level, where

is the value set for the Coarsen by parameter.

enables the use of conservative coarsening techniques that can improve parallel perform-

ance and/or convergence for some difficult cases.

specifies the use of a version of the AMG solver that is optimized for high coarsening rates.

It is recommended if the AMG solver diverges with the default settings.

enables the use of Laplace coefficients when grouping cells for coarsening.

Smoother Type

consist of two types:

is the simplest smoother type and is recommended when using the pressure-based se-

gregated solver.

ILU

is more CPU intensive, but has better smoothing properties for block-coupled systems

such as the pressure-based coupled solver and the density-based implicit solver.

Flexible Cycle Parameters

contains parameters that control the flexible multigrid cycle.

Sweeps

specifies the number of times to apply the smoothing method each time a relaxation is per-

formed.

Max Fine Relaxations

sets the maximum number of relaxations to be performed on the Level  grid (fine grid level).

This parameter eliminates the possibility that the Gauss-Seidel solver will get “stuck” on the

fine grid level, unable to reduce the residuals by the fraction ( ) required by the Termination

criteria.

Max Coarse Relaxations

sets the maximum number of relaxations to be performed on each grid level above Level

(that is, the coarse grid levels).This parameter eliminates the possibility that the Gauss-Seidel

solver will get “stuck” on a coarse grid level, unable to reduce the residuals on that level by

the fraction ( ) required by the Termination criteria. If the iterative solution on a given grid

level is unable to meet the accuracy constraint of the Termination criteria, the correction

equation will be deemed “converged” when this maximum number of relaxations on that

grid level has been performed.

Options

contains additional multigrid parameters.

Verbosity

controls the amount of information that is printed out by the multigrid solver for monitoring

purposes. See Setting the Verbosity (p. ) for details

FAS Multigrid Controls

contains parameters related to the FAS multigrid solver. See Full-Approximation Storage (FAS) Multigrid

in the Theory Guide and Setting FAS Multigrid Parameters (p. ) for details. As noted in the title of

this dialog box section, the FAS multigrid solver is used only for the Flow equations (pressure, mo-

mentum, and energy).

This section of the dialog box appears only when the density-based explicit solver is used.

contains parameters that control the V,W, and F cycles of the FAS multigrid solver.

sets the number of iterations of the multi-stage solver to be performed on a given grid level

before proceeding to a coarser grid level (the value of

described in Multigrid Cycles in the

Theory Guide).Typically, this is set to .

sets the number of multigrid cycles to be performed on a given grid level before proceeding

back up to the finer grid level (the value of

described in Multigrid Cycles in the Theory

Guide). A value of  results in V-cycle multigrid, and a value of  results in W-cycle multigrid.

contains parameters that control the grouping of cells in the FAS multigrid algorithm.

sets the maximum number of grid levels to be used in the multigrid process. A value of

disables multigrid (no coarse grid levels). If the coarse grids do not already exist, they are

created automatically when you start iterating; you cannot create them by clicking the OK

button. See Turning On FAS Multigrid (p. ) for details.

Coarsen by

controls the number of cells in each successively coarser grid level. By default, this parameter

is set to , indicating that the number of cells on each level will be / of the number on the

previous level. In general, the number of cells on each coarser grid level will be equal to /

of the number on the previous level, where  is the value set for the Coarsen by parameter.

Relaxation Factors

are provided to moderate and stabilize the multigrid corrections.

Courant Number Reduction

sets the factor by which to reduce the Courant number for coarse grid levels (that is, every

level except the finest). Some reduction of time step (such as the default .) is typically re-

quired because the stability limit cannot be determined as precisely on the irregularly shaped

coarser grid cells.

Correction Reduction

sets the factor by which to reduce the magnitude of the multigrid corrections transferred

from one level to the next finer level. A typical value with

is .. If two Pre-Sweeps and

two Post-Sweeps are performed, this value can often be increased to . (that is, full correction

transfer).

Species Correction Reduction

sets the factor by which to reduce the magnitude of the species corrections to stabilize the

multigrid calculation.This item appears only when species transport is being modeled.

Correction Smoothing

sets the correction smoothing factor used to interpolate corrections from a coarser grid to a

finer grid. For multigrid on structured meshes, corrections can be interpolated up to a finer

mesh “smoothly” by using, for example, tri-linear interpolation. For unstructured meshes there

is no analogous simple, algebraic procedure that can be used to interpolate without introducing

substantial high frequency “noise”. Instead, the corrections are first interpolated, and then

subjected to a smoothing pass.The default Correction Smoothing value of . should be

acceptable for all cases; you should not need to change it.

Options

Verbosity

purposes.

Multi-Stage

tab allows you to set parameters that govern the operation of the multi-stage solver. It is available

only when the density-based explicit solver is used. See Changing the Multi-Stage Scheme (p. ) for

Controls

Number of Stages

is the number of stages used in the multi-stage scheme.The default scheme is a -stage scheme

Controls

with coefficients of ., ., and . for the first through third stages, respectively. Although

the dialog box limits the maximum number of stages to five, you can define a scheme with an

arbitrary number of stages with the solve/set/multi-stage text command.

Stage

labels the stage to which the parameters in the other columns apply.

sets the multi-stage coefficient for each stage. Coefficients should be greater than zero and less

than one.The final stage should always have a coefficient of .

Dissipation

sets the stages for which artificial dissipation is evaluated. If a Dissipation box is selected for a

particular stage, artificial dissipation will be updated on that stage. If not selected, artificial dissip-

ation will remain “frozen” at the value of the previous stage.

Viscous

sets the stages for which viscous stresses are evaluated. If a Viscous box is selected for a particular

stage, viscous stresses will be updated on that stage. If not selected, viscous stresses will remain

“frozen” at the value of the previous stage.Viscous stresses should always be computed on the

first stage, and successive evaluations will increase the “robustness” of the solution process, but

will also increase the expense (that is, increase the CPU time per iteration). For steady problems,

the final solution is independent of the stages on which viscous stresses are updated.

Default

sets the fields to their default values, as assigned by ANSYS Fluent. After execution, the Default

button becomes the Reset button.

Reset

Default

Reset

resets the fields to their most recently saved values (that is, the values before Default was selected).

Expert

tab contains specialized parameters for limiting spatial discretization, as well as controls for the non-

iterative solver.

Controls

Spatial Discretization Limiter

contains controls for limiting the spatial discretization. See Selecting Gradient Limiters (p. ) for

more information about limiters.

Limiter Type

selects the type of limiter applied to the spatial discretization: Standard, Multidimensional,

or Differentiable.

Cell to Face Limiting

is where the limited value of the reconstruction gradient is determined at the cell face centers.

Cell to Cell Limiting

is where the limited value of the reconstruction gradient is determined along a scaled line

between two adjacent cell centroids. On an orthogonal mesh (or when the cell-to-cell direction

is parallel to face area direction), this method becomes equivalent to the default cell to face

method. For smooth field variation, cell to cell limiting may provide less numerical dissipation

on meshes with skewed cells.

Apply Limiter Filter

enables the limiter filter.The limiter filter is only available with the Standard and Differentiable

limiter types.

Pseudo Transient Method Usage

allows you to select and modify the parameters for each individual equation. See Setting Solution

Controls for the Pseudo Transient Method (p. )  for details.

On/Off

On/Off

enables/disables the equation-specific steady state solution method for a particular equation.

allows you to use the standard steady state method by turning off pseudo transient for that

particular equation. Specify the corresponding under-relaxation factor to be employed with

a particular equation.

Time Scale Factor

allows you to specify a factor that scales the pseudo time step employed for the flow equations

specified in the Run Calculation task page. A time scale factor other than . (default) allows

the use of an equation specific time step in lieu of using a uniform global pseudo time step.

Non-Iterative Solver Controls

contain parameters that control the sub-iterations for the individual equations. See Time-Advance-

ment Algorithm in the Theory Guide for details.

Max. Corrections

provide control over the maximum number of sub-iterations for each individual equation.

Correction Tolerance

defines the overall accuracy.

Residual Tolerance

controls the solution of the linear equations.

Default

Reset

resets the fields to their most recently saved values (that is, the values before Default was selected). After

execution, the Reset button becomes the Default button.

The Solution Initialization task page allows you to define values for flow variables and initialize the

flow field to these values. See for details about using this dialog box.

Controls

Initialization Method

allows you to choose between Hybrid Initialization and Standard Initialization.

is a collection of boundary interpolation methods, where variables, such as temperature, turbulence,

species fractions, volume fractions, and so on, are automatically patched based on domain averaged

values or a particular interpolation recipe (see Hybrid Initialization (p. )).

Standard Initialization

allows you to define values for flow variables and initialize the flow field to these values.

is a drop-down list of zones; the default values for applicable variables will be computed from information

contained in the zone that you select from this list.The computation will occur when you select the required

zone, and the variable values will be displayed in Initial Values.You can also choose the all-zones item

in this list to compute average values based on all zones.

indicates whether the initial velocities are absolute velocities (Absolute) or velocities relative to the motion

of each cell zone (Relative to Cell Zone).This selection is necessary only if your problem involves moving

reference frames or sliding meshes. If there is no zone motion, both options are equivalent.

Initial Values

displays the initial values of applicable variables.You can use Compute from to compute values from a

particular zone, or you can enter values directly. For species transport cases with a single phase flow, only

the boundary species that you have selected in the Select Boundary Species dialog box (see Figure . :The

Select Boundary Species Dialog Box (p. )) appear in the list.You can add or remove a species using the

Select Boundary Species dialog box that can be accessed by clicking Species in the Initialization task

page.

initializes the entire flow field to the values listed.

Initialize Acoustics...

opens the Acoustics Initialization Dialog Box (p. ).

Reset

resets the fields to their “saved” values.

Patch...

opens the Patch Dialog Box (p. ).

Species

Box (p. )), where you can select the boundary species to be displayed in the Initial Values list and in

the Patch, Hybrid Initialization, and relevant boundary conditions dialog boxes.You can modify the se-

lected boundary species list on the fly during the problem setup.This item appears for species transport

cases with a single phase flow only.

allows you to reset the interphase sources/sinks of momentum, heat, and/or mass to zero.This item is

available when you perform coupled discrete phase calculations. See Resetting the Interphase Exchange

Terms (p. ) for details.

can be used to both initialize the flow statistics and reset the flow statistics after you have gathered some

data for time statistics.This item is available when you perform unsteady calculations and have enabled

Solution Initialization Task Page

the Data Sampling for Time Statistics option in the Run Calculation Task Page (p. ). See User Inputs

for Time-Dependent Problems (p. ) for details.

VOF Check

prints a summary report for the VOF case setup.This button is displayed only for VOF multiphase cases. It

becomes available after the case is initialized. For details, see Multiphase Case Check (p. ).

opens the Hybrid Initialization Dialog Box (p. ).This button is available only when Hybrid Initialization

is the selected method.

... Acoustics Initialization Dialog Box

... Patch Dialog Box

... Hybrid Initialization Dialog Box

The acoustics initialization dialog box allows you to initialize/reinitialize the solution of the acoustics

wave equation and to specify how long to ramp acoustic sources.

Controls

Number of Timesteps for Ramping of Sources

sets how many timesteps the sound sources will ramp to their full values.

The Patch dialog box allows you to patch different values of flow variables into different cells. See

Patching Values in Selected Cells (p. ) for details about using this feature.

Controls

indicates whether patched velocities are absolute velocities (Absolute) or velocities relative to the motion

reference frames or sliding meshes. If there is no zone motion, both options are equivalent. Also, this se-

lection affects only velocities, so the options will not be available unless you have selected a velocity in

the Variable list.

Phase

contains a list of all of the phases in the problem that you have defined.This is available when the VOF,

mixture, or Eulerian multiphase model is enabled.

Variable

contains a list of flow variables from which you can choose the variable to be patched. For species transport

cases with a single phase flow, only the boundary species that you have selected in the Select Boundary

Species dialog box (see Figure . :The Select Boundary Species Dialog Box (p. )) appear in the list.

You can add or remove a species using the Select Boundary Species dialog box that can be accessed

by clicking Species in the Initialization task page.

Volume Fraction Patch Options

contains options that can be used when patching volume fraction for VOF and Eulerian multiphase with

Multi-Fluid VOF simulations.

applies a piecewise-linear reconstruction of the interface when patching a user-defined register and

patches cells that intersect the interface with the actual volume fraction.

enables smoothing of the volume fraction based on the volumetric average over the cell neighbors.

After enabling volumetric smoothing, you can click Smooth to apply smoothing to the volume fraction

field for all phases in the entire domain.

Smoothing Relaxation Factor

controls the degree of smoothing applied to the volume fraction field.This can be set between  (no

smoothing) and  (maximum smoothing).

Value

sets a constant value to be patched for the selected Variable.

Value

Use Field Function

enables the patching of a custom Field Function, rather than a constant Value, for the selected Variable.

See Using Field Functions (p. ) for details.

Field Function

contains a list of defined custom field functions. If the Use Field Function option is enabled, you can

patch one of these functions for the selected Variable. See Using Field Functions (p. ) for details.

Zones to Patch

contains a list of cell zones.The specified Value or Field Function for the selected Variable will be

patched into the zones you select from this list.

Registers to Patch

contains a list of cell registers that have been created using the adaption tools.You can patch a different

value for a group of cells within a single cell zone by selecting a register containing a subset of the cells

in the zone. See Using Registers (p. ) for details.

Patch

updates the flow-field data based on the inputs above.

Smooth

apply volumetric smoothing to the volume fraction field.This button only appears if Volumetric

Smoothing is enabled.

The Hybrid Initialization dialog box contains a host of adjustable settings that control the Hybrid

Initialization strategy.

Controls

General Settings

allow you to adjust such entries as the number of iterations and under-relaxation factors.

uses a default value of .This is the number of iterations that will be performed while solving the

Laplace equations to initialize the velocity and pressure. If the initialized velocity and pressure fields

are not to your liking, you may want to increase the number of iterations and re-initialize the solution.

uses a default value of .This value will be used while solving the Laplace equation to initialize the

velocity and pressure. If the initialized velocity and pressure fields are not to your liking, you may

want to adjust the under-relaxation factor and re-initialize the solution.

indicates whether the initial velocities are absolute velocities (Absolute) or velocities relative to the

motion of each cell zone (Relative to Cell Zone).This selection is necessary only if your problem in-

volves moving reference frames or sliding meshes. If there is no zone motion, both options are equi-

valent.

Initialization Options

allows you to include any of the three initialization options.

Use Specified Initial Pressure on Inlets

if you want the specified pressure for Supersonic/Initialization Gauge Pressure at the inlet

boundaries to be used for solving the Laplace equation for the pressure.

Use External-Aero Favorable Settings

if you want to have the velocity potential patched with a linear value to help accelerate conver-

gence of Scalar Equation– and to obtain a better guess of the velocity field for external-aero

problems.

Maintain Constant Velocity Magnitude

if you want to use the flow direction obtained from solving the velocity potential (Scalar Equa-

tion–), while maintaining a constant velocity magnitude throughout the computational domain.

Turbulence Settings

uses by default the domain averaged values for the turbulence parameters. If you want to use variable

turbulence parameters you can deselect the Average Turbulent Parameters check box.When this option

is disabled, then it calculates the turbulent parameters, such as kinetic energy, dissipation energy, and

so on, using local flow parameters.

Species Settings

will by default initialize secondary species with zero mass or mole fractions. If you want to specify the

appropriate value for the species, you must enable Specify Species Parameters. Note that only the

boundary species that you have selected in he Select Boundary Species dialog box (see Figure . :The

page.

The Calculation Activities task page allows you to set up various tasks that you can perform during

the calculation, such as saving files, exporting files, creating solution animations, and command execution.

Controls

Autosave Every

allows you to set the frequency of the autosave.

Edit...

opens the Autosave Dialog Box (p. ).

Automatic Export

displays a list of available export objects that will be executed during the calculations.This list and its as-

sociated buttons are only available for transient flow calculations.

Calculation Activities Task Page

Create

provides a drop-down list that contains options for creating export objects.Two options are available:

Create

the Solution Data Export option opens the Automatic Export Dialog Box (p. ); the Particle History

Data Export option opens the Automatic Particle History Data Export Dialog Box (p. ).

Edit...

opens the appropriate dialog box for the selected item in the Automatic Export list.

Delete

removes the selected item from the Automatic Export list.

Execute Commands

lists available commands to be executed during the calculations.

opens the Execute Commands Dialog Box (p. ).

allows you to automatically have your solution initialized and your case file modified.

Edit...

opens the Automatic Solution Initialization and Case Modification Dialog Box (p. ).This button is

only available when the Automatically Initialize Solution and Modify Case option is enabled.

... Autosave Dialog Box

... Data File Quantities Dialog Box

... Automatic Export Dialog Box

... Automatic Particle History Data Export Dialog Box

... Execute Commands Dialog Box

... Define Macro Dialog Box

... Automatic Solution Initialization and Case Modification Dialog Box

The Autosave dialog box allows you to specify automatic saving of case and data files at specified

intervals during a calculation. See Automatic Saving of Case and Data Files (p. ) for details.

Controls

Save Data File Every

specifies the frequency with which data files are saved. For steady flows you will specify the frequency

Controls

in iterations, while for unsteady flows you will specify it in either time steps or flow time (unless you are

using the explicit time stepping formulation, in which case you will specify the frequency in iterations or

if you are running an in-cylinder simulation you can specify the frequency in crank angles).The default

value is set to zero, indicating that no automatic saving is performed.

Save Associated Case Files

gives you the choice to save the case file only if it is modified or each time that the data file is saved.

Only if Modified

results in ANSYS Fluent saving a case file only if there is a change in the case file settings.

Each Time

allows you to save the case file every time the data file is saved.

Important

When the Retain Only the Most Recent Files option is selected, the solution history

currently in memory will be discarded and the solution history reset.

Data File Quantities

opens the Data File Quantities Dialog Box (p. ) where you can specify which quantities you want to

automatically save to a data file for postprocessing.

File Name

specifies the root name for the files that are saved.The iteration or time-step number and an appropriate

suffix (.cas or .dat) will be added to the specified root name. If the specified File Name ends in .gz

or .Z, appropriate file compression will be performed. (See Reading and Writing Compressed Files (p. )

for details about file compression.)

allows you to select flow-time, time-step, or crank-angle to be appended to the file name.This option

is available only for unsteady-state calculations (only for in-cylinder calculations in the case of crank-

angle).The default selection is flow-time.

Decimal Places in File Name

allows you to specify the number of decimal digits in the file name.This option is available only when

flow-time or crank-angle is selected in the Append File Name with drop-down list.The default value

for this field is set to .

The Data File Quantities dialog box allows you to specify various quantities for postprocessing. See

Setting Data File Quantities (p. ) for details.

Controls

Standard Quantities

contains a listing of standard postprocessing quantities (for example, density, Mach number, temperature,

and so on).

Additional Quantities

Controls

and so on).

contains a listing of additional postprocessing quantities that are derived from the standard quantities

(for example, standard pressure, velocity magnitude, and so on).

The Automatic Export dialog box allows you to create an automatic export definition for solution

data. See Creating Automatic Export Definitions for Solution Data (p. ) for details.

Controls

Name

specifies the name of the export definition.

File Type

contains a drop-down list of file types, which control the output file format that will be written.

ABAQUS

allows you to specify the surface(s) and optional loads, based on the kind of finite element analysis

selected, to be exported to an ABAQUS file (extension .inp).

ASCII

allows you to specify the surface(s), scalars, location from which the values of scalar functions are to

be taken, and the delimiter separating the fields, to be exported to an ASCII file.

AVS

allows you to specify the scalars you want to write to be exported to an AVS file.

CDAT for CFD-Post & EnSight

allows you to specify the cell zones, surfaces, quantities, format (Binary or ASCII), and whether a case

file is written for data export.The .cdat file format is compatible with both CFD-Post and EnSight.

CGNS

allows you to specify the scalars you want to write and the location from which the values of scalar

functions are to be taken, to be exported to a CGNS file (extension .cgns).

allows you to specify the surface(s) and the scalars you want to write to be exported to a Data Ex-

plorer file (extension .dx).

allows you to specify the scalars you want to write, the cell zones, interior zone surfaces, and location

in the cell from which the values of scalar functions are to be taken, and the file format, to be exported

to an EnSight file (extension .geo, .vel, .scl1, or .encas).

FAST

allows you to specify the scalars you want to write, to be exported as a grid file (Plot3D format), a

velocity file, and a scalar file.This option is available only for a triangular or tetrahedral mesh.

FAST Solution

allows you to export a single file containing density, velocity, and total energy data.This option is

available only for a triangular or tetrahedral mesh.

Fieldview Unstructured

allows you to specify the scalars you want to write and the cell zones from which the values of scalar

functions are to be taken, to be exported to a FIELDVIEW binary file (extension .fvuns) and a regions

file (extension .fvuns.fvreg).

I-deas Universal

allows you to specify the surface(s), scalars, and optional loads, based on the kind of finite element

analysis selected, to be exported to an I-deas Universal file.

Mechanical APDL Input

selected, to be exported to a Mechanical APDL Input file (extension .cdb).

NASTRAN

analysis selected, to be exported to a NASTRAN file (extension .bdf).

PATRAN

PATRAN

analysis selected, to be exported to a PATRAN neutral file (extension .out).

TAITherm

allows you to specify the surface(s) for which you want to write data and the method of writing the

heat transfer coefficient, to be exported to a PATRAN neutral file (extension .neu).This option is

available only when the Energy Equation is enabled.

Tecplot

allows you to specify the surface(s) and the scalars you want to write, to be exported to a Tecplot file.

Cell Zones

specifies the cell zones for which data is to be written for a CFD-Post compatible, EnSight, or FIELDVIEW file.

Surfaces

specifies the surfaces for which data is to be written for an ABAQUS, ASCII, Data Explorer, I-deas Universal,

Mechanical APDL Input, NASTRAN, PATRAN,TAITherm, or Tecplot file.

specifies valid quantities for output.The attributes of the list are modified based on the active file type.

The list may be a single-selection or a multiple-selection list or it may be disabled, depending on the se-

lected File Type.

Analysis (for ABAQUS, I-deas Universal, Mechanical APDL Input, NASTRAN, and PATRAN formats)

specifies the finite element analysis intended.

Structural

specifies structural analysis and allows you to select the Structural Loads to be written.

Thermal

specifies thermal analysis and allows you to select the Thermal Loads to be written.

Structural Loads

contains optional structural loads that can be written to ABAQUS, I-deas Universal, Mechanical APDL Input,

NASTRAN, and PATRAN files.This option is available only when Structural analysis is selected.

Force

enables force to be written as a load for a structural analysis.

Pressure

enables pressure to be written as a load for a structural analysis.

enables temperature to be written as a load for a structural analysis.This option is available only when

the Energy Equation is enabled.

Thermal Loads

contains optional thermal loads that can be written to ABAQUS, I-deas Universal, Mechanical APDL Input,

NASTRAN, and PATRAN files.This option is available only when Thermal analysis is selected.

enables temperature to be written as a load for a thermal analysis.

Heat Flux

enables heat flux to be written as a load for a thermal analysis.

Heat Trans Coeff

enables heat transfer coefficient to be written as a load for a thermal analysis.

Location (for ASCII, CGNS, and EnSight Case Gold formats)

specifies the location from which the values of scalar functions are to be taken.

Node

specifies that data values at the node points are to be exported.

Cell Center

specifies that data values from the cell centers are to be exported.

EnSight Parallel

(Available only with Fluent in parallel) creates .encas files suitable for use in EnSight Enterprise.

Format (for CDAT for CFD-Post & EnSight and EnSight Case Gold)

specifies the file format.

Binary

specifies the file format as binary.

ASCII

specifies the file format as ASCII.

Heat Transfer Coefficient (for TAITherm format only)

specifies the basis for the heat transfer coefficient exported.

Flux Based

specifies the flux based method for writing the heat transfer coefficient.

Wall Function

Flux Based

specifies the wall function based method for writing the heat transfer coefficient.

Write Case File Every Time (for CDAT for CFD-Post Y EnSight)

specifies whether a case file is written with every .cdat file, or if case files are written based on the settings

specified by the file/transient-export/settings/cdat-for-cfd-post-&-ensight text

command.

Export Data Every

specifies the frequency for appending the data during the solution process based on either Time Steps

or Flow Time.

File Name

specifies the root name for the files to be saved.

allows you to select flow-time or time-step to be appended to the file name.

flow-time is selected in the Append File Name with drop-down list.The default value for this field is set

to .

The Automatic Particle History Data Export dialog box allows you to create an automatic particle

history export definition for solution data. See Creating Automatic Export Definitions for Transient

Particle History Data (p. ) for details.

Controls

Name

specifies the name of the particle history export definition.

File Type

specifies the type of the file you want to write.

CFD-Post

allows you to write the file in CFD-Post particle tracks format, which can be read in CFD-Post.

FieldView

allows you to write the file in FIELDVIEW format, which can be read in FIELDVIEW.

EnSight

FieldView

EnSight

allows you to write the file in EnSight format.

allows you to select the required injection from the list of predefined injections.

Quantity

contains the list of variables for which you can export the particle data.

Skip

allows you to “thin” or “sample” the number of particles that are exported.

Frequency (Time Steps) or (DPM Iterations)

specifies the frequency of particle time steps that are used for saving the export file.

Separate Files for Each Time Step

allows you to have separate exported data files for each time step. Available only when EnSight is selected

as the File Type.

Particle File Name

allows you to specify the file name/directory for the exported data, using the Browse... button.

Ensight Encas File Name

is the file name you will specify if you selected EnSight under File Type. Use the Browse... button to

select the .encas file that was created when you exported the file with the File/Export... ribbon tab

option.

The Execute Commands dialog box allows you to define commands to be executed during the calcu-

lation. See Executing Commands During the Calculation (p. ) for details about using this feature.

Controls

Defined Commands

sets the total number of monitor commands to be defined.

Active

activates/deactivates the execution of each command.

Name

specifies a name for each command.

Every,When

indicate how often the command is to be executed.You can enter the interval under Every and select

Name

Iteration, Time Step or Flow Time under When. (Time Step and Flow Time are only valid choices if you

are calculating unsteady flow.)

Command

specifies the command to be executed.You can enter text commands or the name of a command macro

that you have defined in the Define Macro Dialog Box (p. ).

Define Macro...

opens the Define Macro Dialog Box (p. ), in which you can define command macros.

End Macro

ends the definition of a macro. (This button will replace the Define Macro... button when you click OK

in the Define Macro dialog box.)

The Define Macro dialog box allows you to define macros for automatic execution by the command

monitor, or for interactive use by you. See Defining Macros (p. ) for details.

Controls

Macros

contains a selectable list of the currently-defined macros.

Name

specifies a name for the command macro.

The Automatic Solution Initialization and Case Modification dialog box allows you to specify the

solution initialization method and to modify the case. See Automatic Initialization of the Solution and

Case Modification (p. ) for details.

Controls

tab contains several choices for initializing the solution.

Use Solution Data From File

requires you to read in a data file containing the desired initialization for the case.

Use Solution Data From Previous Parametric Run with Workbench

(transient cases only) requires you to select one of two methods to initialize the first run.You can

Initialize with Values from the Case, which uses the values set in the Solution Initialization task

page. Otherwise, you can Use Solution Data from File, which requires you to read in a data file

containing the desired initialization for the case.

is analogous to changing the values in a case and continuing the calculation. However, the iteration

counter will be reset to  so that the modifications can be applied. Use this method when no solution

data exists, similar to the first run.

Case Modification

allows you to indicate how long you would like to run with the original settings, then make any modific-

ations to the case settings.

Defined Modifications

indicates the number of modifications for the case file.

Active

allows you to enable or disable a defined case modification.

Name

represents the name of the case modification.

Commands

represents an area where you can enter text commands.

Number of Iterations/Time Steps

represents the number of iterations or time steps that you want to run defined case modification

commands.

The Run Calculation task page allows you to start the solver iterations. See Performing Steady-State

Calculations (p. ) and Performing Time-Dependent Calculations (p. ) for details about the items

below.

Controls

below.

Controls

opens the Case Check Dialog Box (p. ).

opens the Mesh Motion Dialog Box (p. ) for transient simulations.

Update Dynamic Mesh...

opens the Mesh Motion Dialog Box (p. ) for steady simulations.

Run Calculation Task Page

Pseudo Transient Settings

is available for fluid and solid zones and will only appear for steady-state cases, where the pressure-based

coupled solver is used. Note that the Pseudo Transient option must be enabled in the Solution Methods

Task Page (p. ). For details about the available options, see Solving Pseudo-Transient Flow (p. ).

(for steady flow calculations) contains settings for running, reporting, and updating the calculation.

sets the number of iterations to be performed.

sets the number of iterations that will pass before convergence monitors will be printed and plotted.

The default is  (that is, reports will be updated after each iteration).

Profile Update Interval

sets the number of iterations that will pass before user-defined functions for boundary profiles will be

updated.

Time Advancement

(for transient flow calculations) contains settings related to time advancement.

Type

allows you to specify the type of time stepping from the following selections.The type you select will

determine what further selections are available in the Method drop-down list.

Fixed

specifies that the time step size is fixed to a user-specified value or a value based on a specified

period or frequency.

Adaptive

specifies that the time step size changes during the solution, in order to either satisfy the Cour-

Adaptive

ant–Friedrichs–Lewy (CFL) condition, maintain a certain truncation error associated with the time

integration scheme, or satisfy criteria that is specific for multiphase simulations.

User-Defined Function

specifies that the time step size is defined by a user-defined function that uses the DEFINE_DELTAT

macro.

Method

allows you to select one of the following, to specify how the time step is determined:

User-Specified

(for the Fixed type) selects a fixed time step, equal to the specified Time Step Size.

Period-Based

(for the Fixed type) allows you to specify a period (in seconds) as the basis for determining the

time step size and number of time steps. See User Inputs for Time-Dependent Problems (p. )

Frequency-Based

(for the Fixed type) allows you to specify a frequency (in hertz) as the basis for determining the

CFL-Based

(for the Adaptive type) selects a time step that gets modified by ANSYS Fluent as the calculation

proceeds such that the Courant–Friedrichs–Lewy (CFL) condition is satisfied, using the specified

Courant Number. See CFL-Based Time Stepping (p. ) for details.

Error-Based

(for the Adaptive type) selects a time step that gets modified by ANSYS Fluent  based on the

specified truncation Error Tolerance. See Error-Based Time Stepping (p. ) for details.

Multiphase-Specific

convective time scale (Global Courant Number): the time-step-size calculation depends on the

using the implicit or explicit volume fraction formulation, except for the wet steam model. See

Multiphase-Specific Time Stepping (p. ) for details.

Duration Specification Method

(for the Adaptive or User-Defined Function type) specifies the way in which you will define the cal-

culation duration.The duration can be defined by the total time, the total number of time steps, the

incremental time, or the number of incremental time steps. In this context, "total" indicates that Fluent

will consider the amount of time / steps that have already been solved and stop appropriately,

whereas "incremental" indicates that the solution will proceed for a specified amount of time / steps

regardless of what has previously been calculated.

(for transient flow calculations) contains settings for running, reporting, and updating the calculation.

sets or reports the number of time steps to be performed.

Period

sets or reports the period to be used in time step calculation.

Frequency

sets or reports the frequency to be used in time step calculation.

Time Steps per Period

sets the number of time steps to divide each period into.

Total Periods

sets the number of periods for the simulation to run.

Total Time

sets the total time that will be calculated, including the time for which results were generated

during previous calculations.

Total Number of Time Steps

Total Time

sets the total number of time steps to be performed, including the number of time steps performed

in previous calculations.

Incremental Time

sets the incremental time (that is, the additional time) for which results are to be calculated.

sets or reports the magnitude of the (physical) time step

.

allows you to specify the Courant number for CFL-based time stepping.The default value for the

Courant number is .

specifies the threshold value to which the computed truncation error is compared as part of error-

based time stepping. Increasing this value will lead to an increase in the size of the time step and

a reduction in the accuracy of the solution. Decreasing it will lead to a reduction in the size of the

time step and an increase in the solution accuracy, although the calculation will require more

computational time. For most cases, the default value of . is acceptable.

allows you to specify the global Courant number for multiphase-specific time stepping.The default

value for the Global Courant number is .

User-Defined Time Step

contains a drop-down list of available user-defined functions (UDFs) that can be used to define

the time step size.

Number of Fixed Time Steps

specifies the number of fixed-size time steps that should be performed before the size of the time

step starts to change.The size of the fixed time step is the value specified for Initial Time Step

Size.

Size.

is used for the first time step and then for as many subsequent steps as specified in the Number

of Fixed Time Steps field.This value must fall between the minimum and maximum time step

sizes. For a better startup, it should be chosen such that the Courant number initially remains close

to  or your specified value (whichever is lower). Note that if you initialize the solution for a previ-

ously run case with adaptive time stepping, then ANSYS Fluent will use the time step size saved

in the case.

Max Iterations/Time Step

(when using an implicit unsteady formulation) sets the maximum number of iterations to be per-

formed per time step. If the convergence criteria are met before this number of iterations is per-

formed, the solution will advance to the next time step. See User Inputs for Time-Dependent

Problems (p. ) for details.

sets the number of time steps that will pass before convergence monitors will be printed and

plotted.The default is  (that is, reports will be updated after each time step).

sets the number of time steps that will pass before user-defined functions for boundary profiles

Time Step Size Update Interval

specifies the number of time steps that will pass before the time step size is updated for adaptive

time stepping methods.

opens the Adaptive Time Stepping Dialog Box (p. ), so that you can define further settings for

the adaptive time stepping method.

Options

contains options related to unsteady calculations.

Extrapolate Variables

Options

instructs ANSYS Fluent to predict the solution variable values for the next time step and then input

that predicted value as an initial guess for the inner iterations of the current time step.

Report Simulation Status

opens the Simulation Status Dialog Box (p. ), which reports details about the simulation.

Specify Solid Time Step Size

enables a different time step size to be specified for solid zones, either user specified or automatically

calculated.This option is only available when there is a solid zone in the domain and energy is enabled.

See Specifying a Solid Time step (p. ) for details.

Method

specifies how the time step size is determined for solid zones.

specifies the time step size for solid zones when you have selected User-Specified for the Method.

Options

contains options for steady-state simulations that use the density-based implicit solver.

allows you to set parameters that will help ANSYS Fluent guide the calculations to a converged solution.

This option is only available for steady-state simulations that use the density-based implicit solver. See

Solution Steering (p. ) for more information.When enabled, the following options are available:

Flow Type

allows for full multigrid initialization.

The blending factor will be grayed out if Second Order Upwind discretization for the Flow equations

is not selected in the Solution Methods task page.The solution accuracy may be reduced (typical

values are % or %) if it is not possible to obtain a converged solution with the maximum second-

order accuracy (blending = %).

opens the Solution Steering Dialog Box (p. ).

is a non-adjustable field displaying the current CFL number, which allows you to view it during the

Solution Processing

contains controls related to the processing of the calculations.

Acoustic

contains controls for simulations that use the FW-H acoustics model.

Time Step Size for Acoustic Data Export

determines the highest frequency that the acoustic analysis reproduces.This is available for the

density-based solver when both the explicit formulation and explicit transient formulation are se-

lected.

Acoustic Sources FFT...

opens the Acoustic Sources FFT Dialog Box (p. ).This button is only available for three-dimen-

sional transient simulations, when the Export Acoustic Source Data in ASD Format option is

enabled in the Acoustics Model dialog box.

Acoustic Signals...

opens the Acoustic Signals Dialog Box (p. ).

Pollutants

contains controls for simulations that model pollutant formation.

Postprocess Pollutants

results in the automatic postprocessing of pollutants during a transient simulation.

Max Post Iterations/Time Step

sets the maximum number of postprocessing iterations to be performed per time step.This field

is available when the Postprocess Pollutants option is enabled.

PDF Transport Time Averaging

contains solution controls for steady-state simulations that use the composition PDF transport model

with the Lagrangian method.

Iterations in Average

specifies the number of iterations included in the PDF transport time averaging. For recommend-

ations on how to use this setting, see Monitoring the Solution (p. ).

Iteration Increment

specifies the rate at which the number of iterations included in the PDF transport time averaging

will increase in each subsequent iteration. For recommendations on how to use this setting, see

Monitoring the Solution (p. ).

Statistics

contains controls for sampling statistics.

enables the sampling of data during a steady-state calculation. See Performing Steady-State Calcu-

lations (p. ) and Postprocessing for Time-Dependent Problems (p. ) for details.

enables the sampling of data during an unsteady calculation. See User Inputs for Time-Dependent

Problems (p. ) and Postprocessing for Time-Dependent Problems (p. ) for details.

Sampling Interval

allows you to specify the frequency of the Data Sampling for Steady Statistics or Data Sampling

for Time Statistics.

Sampled Iterations

reports the number of iterations over which data has been sampled for the postprocessing of the

mean and RMS values.

Sampled Time

reports the time period over which data has been sampled for the postprocessing of the mean

and RMS values.

Sampling Options...

opens the Sampling Options Dialog Box (p. ) for the Data Sampling for Steady Statistics or

Data Sampling for Time Statistics.

Data File Quantities...

opens the Data File Quantities Dialog Box (p. ).

Solution Advancement

contains buttons that advance the solution.

Calculate

starts the calculations.While the calculation is in progress, a progress bar will appear at the bottom of

the Fluent window. For steady-state simulations, clicking the Stop button next to the progress bar will

interrupt the calculation at the earliest safe stopping point after the current iteration; for transient

simulations, buttons are available that allow you to stop the calculation at the end of the current iter-

ation or time step. Alternatively, you can type Ctrl+c in the console; for transient simulations, a single

instance will stop the calculation at the end of the current time step, whereas typing it twice will stop

it at the end of the current iteration.

Continue Calculation

continues the calculations.This button is available when you have enabled the Automatically Initialize

and Modify Case option in the Calculation Activities task page.

Start Calculation Over

restarts the calculation from the beginning.This button is available when you have enabled the

Automatically Initialize and Modify Case option in the Calculation Activities task page.

... Case Check Dialog Box

... Adaptive Time Stepping Dialog Box

... Simulation Status Dialog Box

... Solution Steering Dialog Box

... Acoustic Sources FFT Dialog Box

... Acoustic Signals Dialog Box

... Sampling Options Dialog Box

This function provides you with guidance and best practices when choosing case parameters and

models. Your case will be checked for compliance in the mesh, models, boundary and cell zone condi-

tions, material properties, and solver categories. Established rules are available for each category, with

recommended changes to your current settings. Information about each of the recommendations is

available in Checking Your Case Setup (p. ).

Controls

Mesh

displays recommendations, if any, relating the to the mesh used in the case. See Checking the Mesh (p. )

Models

displays recommendations, if any, relating the to the models used in the case. See Checking Model Selec-

Boundaries and Cell Zones

displays recommendations, if any, relating the to the cell zones or boundaries defined in the case. See

Checking Boundary and Cell Zone Conditions (p. ) for details.

Materials

displays recommendations, if any, relating the to the materials defined in the case. See Checking Material

Properties (p. ) for details.

Solver

displays recommendations, if any, relating the to the solver settings used in the case. See Checking the

Solver Settings (p. ) for details.

The Adaptive Time Stepping dialog box provides additional settings that affect the adaptive time

stepping. See Performing Time-Dependent Calculations (p. ) for details about adaptive time stepping.

Controls

specify the upper and lower limits for the size of the time step. If the time step becomes very small, the

computational expense may be too high; if the time step becomes very large, the solution accuracy may

not be acceptable to you.You can set the limits that are appropriate for your simulation.

limit the degree to which the time step size can change at each time step. Limiting the change results in

a smoother calculation of the time step size, especially when high-frequency noise is present in the

solution. For the CFL-Based and Multiphase-Specific methods, the time step change factor is computed

as the ratio between the current time step and the previous time step. For the Error-Based method, the

time step change factor is computed as the ratio between the specified truncation error tolerance and

the computed truncation error.

The Simulation Status dialog box reports details about the simulation.

Controls

(for adaptive time stepping) reports the size of the last time step calculated for the simulation.

Total Flow Time

reports the total time calculated for the simulation.

Total Time Steps

reports the number of time steps calculated for the simulation.

Total Iterations

reports the number of iterations calculated for the simulation.

Minimum Time Step Size

(for adaptive time stepping) reports the size of the smallest time step used since either the start of the

simulation or the last time you clicked the Calculate button in the Run Calculation task page, depending

on whether you have clicked the Reset Min and Max Status button.

Maximum Time Step Size

(for adaptive time stepping) reports the size of the largest time step used since either the start of the

Reset Min and Max Status

(for adaptive time stepping) resets the Minimum Time Step Size and Maximum Time Step Size fields,

so that they consider only the values since the latest time you clicked the Calculate button in the Run

The Solution Steering dialog box is used to set the parameters that control the solution steering

strategy. Solution steering will typically perform full multigrid (FMG) initialization followed by two iter-

ative stages (Stage  and Stage ). The purpose of Stage  is to navigate the solution from the difficult

initial phase of the solution toward convergence by insuring maximum stability. During this stage, the

solution is advanced gradually from 1st-order accuracy to maximum accuracy (user specified and typ-

ically 2nd-order) at a constant low CFL value. In Stage , the solution is driven hard towards convergence

by regular adjustments of the CFL value to insure fast convergence as well as to prevent possible di-

vergence. In Stage , the residual history is monitored and analyzed through regular intervals to de-

termine if an increase or decrease in CFL value is needed to obtain fast convergence or to prevent

divergence. See Solution Steering (p. ) for details.

Controls

Steering Settings

allows you to modify the steering parameters used in Stages  and .

Stage

allows you to set parameters relating to stage .

Duration

is the number of iterations in stage .The CFL number used during these iterations is set in the

Stage

Update the Courant Number

allows you to update the Courant number either Immediately, or After a specified number of

Courant Number Update Interval

defines the frequency at which the Courant number is updated.

allows you to set the starting (Initial) and maximum allowed (Maximum) Courant number values.

The solution steering algorithm will not allow the solver to exceed the maximum Courant number,

but will allow the solver to use a Courant number less than the initial Courant number if divergence

in the solution has occurred.

allows the solution to be under-relaxed to improve convergence.

Default

resets any changes made to the parameters to their original default values.

FMG Settings

allows you to set FMG parameters. For more information about FMG initialization, refer to Full Multigrid

(FMG) Initialization (p. ).

Number of Multigrid Levels

allows you to set the number of multigrid levels.

Number of Cycles

allows you to set the number of cycles for a selected level.

FMG Courant Number

allows you to set the FMG Courant number.

Default

resets any changes to the original default values.

The Acoustic Sources FFT dialog box allows you to: read pressure signals from the acoustic source

data (ASD) files (see Writing Source Data Files (p. )); compute Fourier spectra of these signals at the

selected point probes and over the entire source zones; create surface variables for visualizing the

spectral properties of the flow pressure signals; and write CGNS files of the spectrum data. See FFT of

Acoustic Sources: Band Analysis and Export of Surface Pressure Spectra (p. ) for details about the

Controls

Storage Area Control

allows you to specify how memory is allocated in the “storage area” (that is, the large memory array that

stores the fields of the pressure histories and the computed fields of the Fourier spectra) when you

compute the FFT fields in the Compute FFT Fields tab.

Overwrite Signals by Spectra

specifies that the Fourier spectra displace in memory the original time signals, so that they are not

kept after the FFT has been computed.

Clean Up Only FFT Results

de-allocates the storage area—so that you can re-compute the FFT without re-reading the pressure

histories—and deletes all variables created through the FFT Surface Variables tab.This button is

only available when the Overwrite Signals by Spectra option is disabled.

Clean Up Entire Storage Area

de-allocates the storage area—so that you can re-read ASD files and re-compute the FFT with a clipped

time range or different window function—and deletes all variables created through the FFT Surface

Variables tab.

Point Probes for Time Signals

allows you to get information about existing point probes and create pressure history files.

Existing Points

lists all of the point probes created through the Point Surface Dialog Box (p. ) that are available for

Print Coordinates

prints in the console the coordinates of the point probe(s) selected in the Existing Points selection

list.

Extract Signals

creates ASCII files that contain the pressure histories of the point probe(s) selected in the Existing

Points selection list.

File Name

specifies a prefix for the names of the files created by the Extract Signals button.

allows you to read pressure histories from the acoustic source data (ASD) files.

Active Source Zones

is a list of the face zones for which you can read acoustic source data.

Source Data Files

is a list of the ASD files you can read.

Load Index File...

updates the Active Source Zones and Source Data Files lists by loading an ASCII index file.

Read

reads the pressure signals from the selected items in the Active Source Zones and Source Data Files

lists.

allows you to compute FFT fields from the pressure signals read through the Read ASD Files tab.

Sampling Data

allows you to reduce the time range of the signal data used to compute the FFT fields.

Clip Time to Range

specifies that the time range of the data sampled is reduced to be between the Min and Max.

Min

specifies the minimum value of the time range of the signal data when the Clip Time to Range

Max

specifies the maximum value of the time range of the signal data when the Clip Time to Range

Time Step

reports the size of the time step at which data was sampled.

Re-Estimate Spectral Resolution

updates the values that are displayed in the Spectral Resolution group box and that are used

to compute the FFT fields, based on the settings in the Sampling Data group box.

Spectral Resolution

displays the number of samples and the expected spectrum properties for the provided signals.

Number of Samples

reports the total number of samples in the specified time range.

Samples Used for FFT

reports the number of samples that will be used for FFT (see Table . : Numbers of Data Points

Supported by the Prime-Factor FFT Algorithm (p. )).

Frequency Min & Step

reports the expected minimum frequency in the spectrum, which is also the expected frequency

step.

Frequency Max

reports the expected maximum frequency in the spectrum.

reports the expected number of Fourier modes in the spectrum.

Window Function

specifies the shape of the window function used to enforce the signal's periodicity. See Window-

ing (p. ) for details.The default is the Hanning window.

Compute

computes the FFT fields based on the settings in the Compute FFT Fields tab.

allows you to create new Fluent variables for postprocessing using the spectrum fields computed through

the Compute FFT Fields tab.

Modes/Frequency Bands

specifies what the created variables will characterize.

specifies that the variables characterize proportional frequency bands corresponding to the

standard technical octaves.

standard technical thirds.

specifies that the variables characterize user-defined equidistant frequency bands.

Set of Modes

specifies that the variables characterize the individual Fourier modes.

Octave Central Frequencies

is a list of the octave central frequencies for which you can Create Fluent variables for postprocessing.

This selection list is available when Octave Bands is selected from the Modes/Frequency Bands

/-Octave Central Frequencies

is a list of the /-octave central frequencies for which you can Create Fluent variables for postpro-

cessing.This selection list is available when /-Octave Bands is selected from the Modes/Frequency

Bands drop-down list.

Frequency Min

specifies the minimum frequency of the set of modes for which you want to Create Fluent variables

for postprocessing.This field is available when Set of Modes or Constant Width Bands is selected

from the Modes/Frequency Bands drop-down list.

specifies the maximum frequency of the set of modes for which you want to Create Fluent variables

Number of Modes to Skip

allows you to “thin” or “sample” the modes for which you want to Create the Fluent variables for

postprocessing.This field is available when Set of Modes is selected from the Modes/Frequency

Band Width

specifies the width of the constant width bands, for which you want to Create the Fluent variables

for postprocessing.This field is available when Constant Width Bands is selected from the

Modes/Frequency Bands drop-down list.

Spectrum Property

displays the type of variables created according to the selected choice in the Modes/Frequency

Surface Pressure Level

is displayed when frequency band is selected from the Modes/Frequency Bands drop-down list,

in order to indicate that the created variables will be the surface pressure level (SPL) fields, in

decibels.

Real and Imaginary Amplitude Parts

is displayed when Set of Modes is selected from the Modes/Frequency Bands drop-down list,

in order to indicate that the created variables will be the real and imaginary parts of the complex

Fourier amplitudes, with a pair of variables per specified mode.

Existing Variables

lists the processed variables that have been created by the Create button, and allows you to make

selections for deletion using the Remove Selected Variables button.

Remove Selected Variables

deletes the processed variables selected in the Existing Variables list from the “storage area” (as

described previously), so that you can analyze more than the maximum of  individual modes or

constant width bands that are allowed to exist at any one time.

Write Area-Avg Data

When selected, and upon clicking Create, Fluent writes the area-averaged pressure data to an ASCII

file in the XY plot file format.

Plot Area-Avg Data

When selected, and upon clicking Create, Fluent plots the area-averaged pressure data in the form

of a bar chart in the graphics window.

Create

creates new Fluent variables for postprocessing (based on your settings in the FFT Surface Variables

tab), updates the Existing Variables selection list, and (when Set of Modes or Constant Width Bands

is selected from the Modes/Frequency Bands drop-down list) prints information in the console.

allows you to write CGNS files of the spectrum data.

Processed Source Zones

is a list of the zones you can export.

Frequency Series

allows you to reduce the exported spectrum data.

Reduce Frequency Series

specifies that the exported spectrum data is reduced to be between the Min and Max.

Min

specifies the minimum of the frequency range to be exported when the Reduce Frequency Series

Max

specifies the maximum of the frequency range to be exported when the Reduce Frequency

Series option is enabled.

Number of Frequencies to Skip

allows you to “thin” or “sample” the frequencies to be exported.

Number of Frequencies per File

specifies the number of frequencies exported in each file. A value should be chosen based on the

Number of Modes field of the Compute FFT Fields tab, in order to avoid creating either extremely

large output files or a large number of very small files.

File Name

File Name

specifies the base file name of the output files.

Write

writes CGNS files of the spectrum data.

The Acoustic Signals dialog box is used to compute and save the sound pressure signals. See Postpro-

cessing the FW-H Acoustics Model Data (p. ) for details about the items below.

Controls

Options

contains the options available for acoustic signal postprocessing.

Write Acoustic Signals

enables the parameters needed to write the sound pressure data to files.

Read Unsteady Acoustic Source Data Files

enables the parameters needed to compute the sound pressure signals using the source data saved

to files.

contains source zones you want to include to compute sound. See Specifying Source Surfaces (p. ) for

details.

Receivers

contains all the receivers for which you can compute sound.

contains all the source data files that you can use to compute sound.

opens the Select File dialog box, in which you can select the index file for your computation.

Write

writes the sound pressure data.This button will appear only when Write Acoustic Signals is selected

Compute/Write

computes and saves the sound pressure data.This button will appear only when Read Unsteady

Acoustic Source Data Files is selected under Options.

opens the Acoustic Receivers Dialog Box (p. ) in which you can define additional receivers.

The Sampling Options dialog box allows you to specify a collection of statistics for: Flow Shear

Stresses, Flow Heat Fluxes, Wall Statistics, DPM Variables, and Custom Field Functions.

Controls

Collect Statistics for...

contains options for the variables you want to be able to postprocess.

Flow Shear Stresses

allows you to enable or disable the flow shear stress statistics for postprocessing.

Flow Heat Fluxes

allows you to enable or disable the flow heat fluxes statistics for postprocessing.

Wall Statistics

allows you to enable or disable the wall statistics for postprocessing.

DPM Variables

allows you to enable or disable DPM variable statistics for postprocessing.

allows you to select the previously defined custom field functions you want to be able to postprocess.

The Results task page introduces you to the main tasks involved in setting up and displaying the results

of your CFD simulation using ANSYS Fluent.

The Graphics and Animation task page allows you to visualize the results of your CFD simulation by

allowing you to set up plots of contours, vectors, pathlines, particle tracks, scene descriptions and an-

imations. See Displaying Graphics (p. ) for more information.

Controls

Graphics

displays a list of the available graphics objects.

You can double-click an item in the Graphics list to open the corresponding dialog box, or you can

select the item in the list and click the Set Up... button.

Mesh

Mesh

selecting this item and clicking the Set Up... button opens the Mesh Display Dialog Box (p. ).

Contours

selecting this item and clicking the Set Up... button opens the Contours Dialog Box (p. ).

Vectors

selecting this item and clicking the Set Up... button opens the Vectors Dialog Box (p. ).

Pathlines

selecting this item and clicking the Set Up... button opens the Pathlines Dialog Box (p. ).

Particle Tracks

selecting this item and clicking the Set Up... button opens the Particle Tracks Dialog Box (p. ).

Set Up...

opens the dialog box corresponding to the selected object in the Graphics list.

Graphics and Animations Task Page

Animations

displays a list of the available animation objects.

You can double-click an item in the Animations list to open the corresponding dialog box, or you

can select the item in the list and click the Set Up... button.

Sweep Surface

selecting this item and clicking the Set Up... button opens the Sweep Surface Dialog Box (p. ).

Scene Animation

selecting this item and clicking the Set Up... button opens the Animate Dialog Box (p. ).

Solution Animation

selecting this item and clicking the Set Up... button opens the Playback Dialog Box (p. ).

Set Up...

opens the dialog box corresponding to the selected object in the Animations list.

opens the Display Options Dialog Box (p. ).

Scene...

opens the Scene Description Dialog Box (p. ).

Views...

opens the Views Dialog Box (p. ).

Lights...

opens the Lights Dialog Box (p. ).

opens the Colormap Dialog Box (p. ).

opens the Annotate Dialog Box (p. ).

Views...

Lights...

... Profile Options Dialog Box

...Vector Options Dialog Box

... Custom Vectors Dialog Box

...Vector Definitions Dialog Box

... Path Style Attributes Dialog Box

... Ribbon Attributes Dialog Box

... Particle Filter Attributes

... Reporting Variables Dialog Box

...Track Style Attributes Dialog Box

... Particle Sphere Style Attributes Dialog Box

... Particle Vector Style Attributes Dialog Box

... Sweep Surface Dialog Box

... Create Surface Dialog Box

... Animate Dialog Box

... Save Picture Dialog Box

... Playback Dialog Box

... Display Options Dialog Box

... Scene Description Dialog Box

... Display Properties Dialog Box

...Transformations Dialog Box

... Iso-Value Dialog Box

... Pathline Attributes Dialog Box

... Bounding Frame Dialog Box

...Views Dialog Box

...Write Views Dialog Box

... Mirror Planes Dialog Box

... Graphics Periodicity Dialog Box

... Camera Parameters Dialog Box

... Lights Dialog Box

... Colormap Dialog Box

... Colormap Editor Dialog Box

... Annotate Dialog Box

The Profile Options dialog box controls the scaling and projection direction of profiles. It is opened

from the Contours Dialog Box (p. ), and you will display the profiles using the Display button in

that dialog box. See Displaying Contours and Profiles (p. ) for details about the items below.

Controls

Reference Value

sets the “zero height” reference value for the profile. Any point on the profile with a value equal to the

Controls

Reference Value will be plotted exactly on the defining surface.Values greater than the Reference Value

will be projected ahead of the surface (in the direction of Projection Dir. and scaled by Scale Factor),

and values less than the Reference Value will be projected behind the surface.

sets the length scale factor for projection. After subtracting off the Reference Value, ANSYS Fluent mul-

tiplies the resulting solution value by the Scale Factor to form a length.

Projection Dir.

sets the direction in which profiles are projected. In 2D, for example, a contour plot of pressure on the

entire domain can be projected in the  direction to form a carpet plot, or a contour plot of  velocity on

a sequence of -coordinate slice lines can be projected in the  direction to form a series of velocity

profiles.

The Vector Options dialog box allows you to set additional parameters for vector displays. It is opened

from the Vectors Dialog Box (p. ). See Vector Plot Options (p. ) for details about the items below.

Controls

In Plane

toggles the display of vector components in the plane of the surface selected for display.This feature is

useful for visualizing components that are normal to the flow. See Drawing Vectors in the Plane of the

Surface (p. ) for details.

Fixed Length

enables the display of vectors that are all the same length. See Displaying Fixed-Length Vectors (p. )

X,Y, Z Component

toggle the display of the Cartesian components of the vectors. See Displaying Vector Components (p. )

Scale Head

Scale Head

controls the size of the arrowhead on vector styles that include heads.

Color

specifies a single color for the display of all vectors. See Displaying Vectors Using a Single Color (p. )

The Custom Vectors dialog box allows you to define custom vectors based on existing quantities.

Any vectors that you define will be added to the Vectors of list in the Vectors Dialog Box (p. ). To

open the Custom Vectors dialog box, click Custom Vectors... in the Vectors dialog box. See Creating

and Managing Custom Vectors (p. ) for details about custom vectors.

Controls

Vector Name

specifies the name of the vector you are defining. Should you decide to change the name after you have

defined the vector, you can do so in the Vector Definitions Dialog Box (p. ), which you can open by

clicking on the Manage... button.

, and  components of the vector. Each drop-down list contains the available field functions.

Define

creates the vector and adds it to the Vectors of list in the Vectors Dialog Box (p. ).

Manage...

opens the Vector Definitions Dialog Box (p. ), which enables you to check, rename, save, load, and

delete custom vectors.

The Vector Definitions dialog box allows you to check, rename, save, load, and delete custom vectors

that you defined in the Custom Vectors Dialog Box (p. ). See Creating and Managing Custom Vec-

tors (p. ) for details about the items below.

Controls

display the ,

Controls

, and  components of the vector.

Vectors

contains a selectable list of custom vectors.When you select a vector, its components will appear in the

X, Y, and Z Component fields, and its name will appear in the Name field.

Name

displays the name of the currently selected vector.You can enter a new name in this box if you want to

rename the vector.

Rename

changes the name of the selected function to the name specified in the Name field.

Delete

deletes the selected vector.

Save...

opens The Select File Dialog Box (p. ), in which you can specify a file in which to save all of the custom

vectors in the Vectors list.

Load...

opens the Select File dialog box, in which you can specify a file from which to read custom vectors (a file

that you saved using the Save... button above).

To modify the line width, cylinder radius or marker size, use the Path Style Attributes dialog box. You

can open this dialog box by clicking the Attributes... button in the Pathlines Dialog Box (p. ). See

Controlling the Pathline Style (p. ) for details about the items below.

Controls

Line Width/Marker Size/Width/

determines the thickness of the pathlines.

Diameter

specifies the diameter of the sphere.This parameter appears only when sphere is selected under Style

in the Pathlines dialog box.

Spacing Factor

controls the spacing of arrows when you use the line-arrows style.

Scale

controls the size of the arrow heads when you use the line-arrows style.

Detail

specifies the detail applied to the graphical rendering of the spheres.This parameter appears only when

Scale

Detail

sphere is selected under Style in the Pathlines dialog box.

To modify the ribbon width and set the scalar field by which to twist the ribbon, use the Ribbon At-

tributes dialog box. You can open this dialog box by clicking the Attributes... button in the Pathlines

Dialog Box (p. ) when the selected Style is ribbon. See Controlling the Pathline Style (p. ) for

Controls

Width

determines the thickness of the ribbon.

Twist Scale

sets the amount of twist for a given field.To magnify the twist for a field with very little change, increase

this factor; to display less twist for a field with dramatic changes, decrease this factor.

Twist By

contains a drop-down list from which you can select a scalar field on which pathline twisting is based.

Min/Max

displays the minimum/maximum value of the scalar field selected in Twist By.

The Particle Filter Attributes dialog box allows you to specify how you would like to filter the particles

being displayed. See Particle Filtering (p. ) for details about the items below.

Controls

Options

contains the filtering options.

Inside

enables the filtering of particles with values between Filter-Min and Filter-Max.

Outside

enables the filtering of particles with values less than Filter-Min or greater than Filter-Max.

Filter by

contains a list from which you can select any field variable, except for Custom Field Functions..., to be

used as a filter variable.

Min/Max

Filter by

Min/Max

displays the minimum and maximum values of the selected field variable.The real number field values

are not editable; they are purely informational.

Filter-Min/Filter-Max

defines the minimum/maximum filter threshold.

The Reporting Variables dialog box allows you to control the particle variables that you include in

your reporting. See Step-by-Step Reporting of Trajectories (p. ) for details about the items below.

Controls

Variables in Report

contains all variables currently in the report.

Remove

removes the selected variable from the report.

Default Variables

restores the default list.

Available Particle Variables

contains the particle variables that are available for you to select.

Add Variables

takes the selected variable from the Available Particle Variables list and adds it to the Variables in

Report list.

Add Color By

adds the Color by variable to the Variables in Report list.

To modify the line width, cylinder radius or marker size, use the Track Style Attributes dialog box.

You can open this dialog box by clicking the Attributes... button in the Particle Tracks Dialog

Box (p. ). See Controlling the Particle Tracking Style (p. ) for details about the items below.

Controls

Line Width/Marker Size/Width

determines the thickness of the particle tracks.

Scale

Scale

To modify the attributes of the particle sphere, use the Particle Sphere Style Attributes dialog box.

Select sphere from the Track Style drop-down list and click the Attributes... button in the Particle

Tracks Dialog Box (p. ) to open the Particle Sphere Style Attributes dialog box. See Controlling

the Particle Tracking Style (p. ) for details about the items below.

Controls

Options

allows you to choose how you would like to specify the particle diameter.

Constant

allows you to specify the diameter as a constant value.

Variable

allows you to select a particle variable to estimate the size of the spheres.

Auto Range

when disabled clips the displayed particles to the values given in Min and Max.

Diameter

specifies the diameter of the sphere.

Scale

allows you to scale the spheres by the factor entered in this field.

Detail

specifies the detail applied to the graphical rendering of the spheres.

Size by

contains a list of variables by which you can estimate the size of your particle.This list is selectable only

when you are using the Variable option.

Min/Max

defines the minimum and maximum values of the selected field variable to display.

To modify the attributes of the vector styles, use the Particle Vector Style Attributes dialog box. See

Controlling the Vector Style of Particle Tracks (p. ) for details about the items below.

Controls

Options

Constant Length

Controls

Options

allows you to specify the vector length as a constant value.

Variable Length

results in a vector length that is based on the variable selected under Length by.

Constant Color

when enabled allows you to select a vector color from the Color drop-down list. Otherwise, the vector

is colored based on the variable selected in the Particle Tracks dialog box (seen in the Mesh Colors

Length

specifies the length of the vector.

Scale

allows you to scale the vectors by the factor entered in this field.

Length to Head Ratio

is the ratio of vector length to vector head size.

Vectors of

contains the particle vector variable to display.

Length by

is used to estimate the length of the vector when the Variable Length option is enabled.

The Sweep Surface dialog box controls the display and animation of mesh, contour, and vector plots

generated on a sweep surface. See Displaying Results on a Sweep Surface (p. ) for details about the

Controls

Sweep Axis

specifies the (X, Y, Z) vector representing the axis along which the surface should be swept.

Display Type

specifies the type of display to be swept through the domain (Mesh, Contours, or Vectors).

opens the Contours Dialog Box (p. ) if Contours is the selected Display Type, or the Vectors Dialog

Box (p. ) if Vectors is the selected Display Type. (This button is not available if Mesh is the selected

Display Type.)

Animation

contains controls for animating the sweep-surface display.

Initial Value, Final Value

Animation

specify the initial and final positions for the animation.

Frames

specifies the number of frames in the animation.

Min Value, Max Value

show the minimum and maximum extents of the domain along the specified Sweep Axis.These values

are updated when you click Compute.

Value

shows the current position at which the requested display is plotted.You can change the value by moving

the slide bar below it, or by entering a new value and pressing the <RETURN> key.

Create...

opens the Create Surface Dialog Box (p. ), where you can create a surface from the currently-displayed

sweep surface.

Animate

animates the display, sweeping the requested display through the domain along the specified axis.

Compute

updates the Min Value and Max Value to reflect the minimum and maximum extents of the domain

along the specified Sweep Axis.

The Create Surface dialog box allows you to save a sweep surface for later use. You can open it by

clicking Create... in the Sweep Surface Dialog Box (p. ). See Displaying Results on a Sweep Sur-

face (p. ) for details about the items below.

Controls

Surface Name

specifies a name for the surface to be created.

The Animate dialog box allows you to specify key frames that define the basic movement of an anim-

ated sequence, and then play back the animation. ANSYS Fluent interpolates between your specified

key frames. See Animating Graphics (p. ) for details about the items below.

Controls

Playback

contains the controls that you use to play back the animation. See Playing an Animation (p. ) for details.

Controls

Playback

Playback Mode

contains a drop-down list of playback options.

Play Once

sets the option to play back frames from Start Frame to End Frame once.

Auto Repeat

sets the option to continually play back frames from Start Frame to End Frame.

Auto Reverse

sets the option to continually play back the images while reversing playback direction after each

set.

Start Frame, End Frame

set the frames at which the animation should begin and end. By changing these numbers you can

view a subset of the frames.

Increment

sets the number of frames to increment the frame-counter by when you use the fast-forward or fast-

reverse buttons.

Frame

shows the number of the frame that is currently displayed, as well as its relative position in the entire

animation. If you slide the bar to a different location, the frame corresponding to the new frame

number will be displayed in the graphics window.

(Tape Player Buttons)

allow you to play the animation forward and backward, fast-reverse and fast-forward the animation,

and stop it.The buttons function in a way similar to those on a standard video cassette player.

Key Frames

contains the controls that you use to define the key frames for the animation. See Creating an Anima-

Frame

sets the number to be assigned to the next key frame added to the list of Keys.

Keys

contains a list of the key frames that have been defined. If you select a key frame in this list, the asso-

ciated scene will be displayed in the graphics window.

Add

creates a key frame with the number shown in Frame for the scene currently displayed in the

Add

Important

Be sure to change the frame number before you add the new key frame so that you

will not overwrite the last key frame that you created.

Delete

deletes the key frame that is selected in the Keys list.

Delete All

deletes all key frames in the Keys list.

Write/Record Format

specifies Key Frames, Picture Files, MPEG, or Video (not available on Windows) as the format in which

to save the animation. See Saving an Animation (p. ) for details about these options.

Picture Options...

opens the Save Picture Dialog Box (p. ), in which you can specify parameters for saving the animation

to picture files.This button is available only when Picture Files is selected as the Write/Record Format.

Write...

opens The Select File Dialog Box (p. ), in which you can specify a name for the animation file and save

it.

Read...

opens the Select File dialog box, in which you can specify the name of the animation file to be read. Note

that the current case and data should contain the surfaces and any other information that the key frame

description refers to. See Reading an Animation File (p. ).

The Save Picture dialog box allows you to set save picture parameters and save picture files of

graphics windows. See Saving Picture Files (p. ) for details on the use of this dialog box.

Controls

Format

allows you to select the format of picture files.

EPS

(Encapsulated PostScript) output is the same as PostScript output, with the addition of Adobe Docu-

Format

EPS

ment Structuring Conventions (v2) statements. Currently, no preview bitmap is included in EPS output.

Often, programs that import EPS files use the preview bitmap to display on-screen, although the ac-

tual vector PostScript information is used for printing (on a PostScript device).You can save EPS files

in raster or vector format.

JPEG

PPM

TIFF

PNG

HSF

AVZ

and interactively manipulate the displayed object. For additional information on the ANSYS Viewer,

refer to ANSYS Viewer User's Guide.

VRML

the ANSYS Fluent graphics window.This format can commonly be used by VR systems and in partic-

ular the 3D geometry can be viewed and manipulated in a web-browser graphics window.

Important

Non-geometric entities such as text, titles, color bars, and orientation axis are not

exported. In addition, most display or visibility characteristics set in ANSYS Fluent,

such as lighting, shading method, transparency, face and edge visibility, and outer

face culling, are not explicitly exported but are controlled by the software used to

view the VRML file.

(Linux systems only) selects a window dump operation for generating the picture.With this format,

you will need to specify the appropriate Window Dump Command.

Coloring

(all formats except Window Dump) specifies the color mode for the picture file.

Color

specifies a color-scale copy.

Gray Scale

specifies a gray-scale copy.

Monochrome

specifies a black-and-white copy.

Important

Most monochrome PostScript devices will render Color images in shades of gray, but

to ensure that the color ramp is rendered as a linearly-increasing gray ramp, you should

select Gray Scale.

File Type

specifies the type of picture file to be saved. See Choosing the File Type (p. ) for details.

Raster

specifies a raster type picture.The supported raster formats are EPS, JPEG, PPM, PostScript, TIFF,

and PNG.

Vector

specifies a vector type picture.The supported vector formats are EPS, PostScript, and VRML.

specifies the resolution or the size (in pixels) of the picture.

Use Window Resolution

uses the resolution of the current graphics window when the image is saved.

DPI

specifies the resolution of EPS and PostScript files in dots per inch (DPI).The default value for DPI is

set to .

Width

specifies the width of the raster picture image.

Height

specifies the height of the raster picture image.

The default value for Width and Height is set to zero, so that the default picture is generated at

the same resolution as the active graphics window.

Options

contains additional options for all picture formats except Window Dump.

Options

Landscape Orientation

specifies the orientation of the picture. If this option is enabled, the picture is made in landscape

mode; otherwise, it is made in portrait mode.

White Background

controls the foreground/background color. If this option is enabled, the foreground and background

colors of graphics windows being saved as pictures will be swapped. Hence, it allows you to save

pictures with a white background and a black foreground, while the graphics windows are displayed

with a black background and white foreground.

Window Dump Command

(Linux systems only) specifies the command to be used to save the picture file, when you select the

Window Dump format. See Window Dumps (Linux Systems Only) (p. ) for details.

Save...

opens The Select File Dialog Box (p. ), in which you can specify a name for the picture file to be saved

and then save the file.The resulting file will contain a picture of the active graphics window.

Apply

saves the current settings. ANSYS Fluent will use these settings when making subsequent pictures.

Preview

applies the current settings to the active graphics window so that you can investigate the effects of dif-

ferent options interactively before saving the final picture.

The Playback dialog box allows you to play back an animation sequence. See Playing an Animation

Sequence (p. ) for details about the items below.

Controls

Playback

contains the controls that you use to play back the selected animation sequence.

Play Once

Controls

Playback

Play Once

set.

Use Stored View

disabling allows you to modify the view during animation playback (In Memory and HSF File 3D

animations only).

Increment

Frame

Replay Speed

controls the playback speed for the animation. Move the Replay Speed slider bar to the left to reduce

the playback speed (and to the right to increase it).

Animation Sequences

contains the controls that you use to define the sequence to be played back.

Sequences

contains a list of the animation sequences that have been defined.

Delete

Sequences

Delete

deletes the animation sequence that is selected in the Sequences list.

Delete All

deletes all animation sequences in the Sequences list.

specifies Animation Frames, Picture Files, or MPEG as the format in which to save the animation. See

Saving an Animation Sequence (p. ) for details about these options.

Write

saves the specified file(s) in the current working directory.

Read...

opens The Select File Dialog Box (p. ), in which you can specify the name of the solution animation file

to be read. See Reading an Animation Sequence (p. ) for details.

The Display Options dialog box provides an interactive mechanism for setting attributes or options

that control how and where a scene is rendered.

Controls

Rendering

allows you to modify characteristics of the display that are related to the way in which scenes are rendered.

See Modifying the Rendering Options (p. ) for details about these items.

Line Width

controls the thickness of lines.The default is .

sets the symbol used for nodes and data points.

Animation Option

contains a drop-down list of animation options: All and Wireframe. Wireframe uses a wireframe

representation of all geometry during mouse manipulation This option is turned on by default.You

should turn it off only if your computer has a graphics accelerator; otherwise the mouse manipulation

may be very slow.

turns double buffering on or off, if it is supported by the driver. Double buffering dramatically reduces

screen flicker during graphics updates. Note that if your display hardware does not support double

buffering and you turn this option on, double buffering will be done in software. Software double

buffering uses extra memory.

allows you to turn off the display of outer faces in wall zones. Outer Face Culling is useful for displaying

other.When you turn on the Outer Face Culling option, the display of a slit wall will show each side

distinctly as you rotate the display.This option can also be useful for displaying two-sided walls (walls

turns hidden surface removal on or off. If you do not use hidden surface removal, ANSYS Fluent will

not try to determine which surfaces in the display are behind others; it will display all of them, and a

cluttered display will result.You should turn this option off if you are working with a 2D problem or

with geometries that do not overlap.

Removal Method

chooses the method to be used for hidden surface removal.These options vary in speed and quality,

depending on the device you are using.The choices are listed below.

is the fastest method if your hardware supports it.The accuracy and speed of this method is

hardware dependent.

Painters

will show fewer edge-aliasing effects than hardware-z-buffer.This method is often used instead

of software-z-buffer when memory is limited.

Timeout in seconds

specifies the value for the timeout.

Graphics Window

allows you to open and close graphics windows. See Opening Multiple Graphics Windows (p. ) for details.

Active Window

indicates the graphics window to be opened, closed, or set active. (A graphics window’s ID is displayed

in its title.)

Open/Close

opens or closes the window with the ID shown in the Active Window box. If the indicated window

is open, the Close button will appear, and if the indicated window is not open, the Open button will

appear.

Set

sets the window with the ID shown in the Active Window box to be the active graphics window. See

Setting the Active Window (p. ) for details.

Lighting Attributes

controls lighting attributes for all lights in the active graphics window. See Adding Lights (p. ) for details.

Lights On

turns all lights in the active graphics window on or off.

Lighting

specifies the method to be used in lighting interpolation: Flat, Gouraud, or Phong. (Flat is the most

Lights On

Lighting

basic method: there is no interpolation within the individual polygonal facets. Gouraud and Phong

have smoother gradations of color because they interpolate on each facet.)

Layout

controls the display of captions, axes and the colormap in the graphics display window. See Changing

the Legend Display (p. ) for details.

Logo

allows you to hide or display the ANSYS logo.

Color

contains a drop-down list of colors that can be used for the logo.The choices are White or Black.

Colormap

enables/disables the display of the color scale.

Colormap Alignment

allows you to adjust the alignment of colormap in the graphics display. Select the side (Top, Bottom,

Left, and Right) from the drop-down list, where you want to align the colormap.

Apply

applies the specified attributes and re-renders the scene in the active graphics window with the new at-

tributes.To see the effect of the new attributes on other graphics windows, you must redisplay them.

Info

prints out information about your graphics driver in the console.

Lights...

opens the Lights Dialog Box (p. ), which allows you to create, delete, and modify directional light

sources.

The Scene Description dialog box allows you to turn overlays on and off, select geometric objects in

the display for modification or deletion, and open dialog boxes that control various characteristics of

the selected object(s). (Note that you cannot use the Scene Description dialog box to control XY plot

and histogram displays.) See Advanced Scene Composition (p. ) for details about the items below.

Controls

Names

contains a list of the geometric objects that currently exist in the scene (including those that are presently

invisible).You can specify the object or objects to be manipulated by selecting names in this list. If you

select more than one object at a time, any operation (transformation, color specification, and so on) will

apply to all the selected objects.You can also select objects by clicking on them in the graphics display

using the mouse probe button, which is, by default, the right mouse button. (See Controlling the Mouse

Button Functions (p. ) for information about mouse button functions.) To deselect a selected object,

simply click its name in the Names list. See Selecting the Object(s) to be Manipulated (p. ) for details.

Geometry Attributes

contains information about the type of the selected geometric object and push buttons that open dialog

boxes for modifying the object.

Type

reports the type of the selected object. Possible types include mesh, surface, contour, vector,

and Group.This information is especially helpful when you need to distinguish two or more objects

with the same name.When more than one object is selected, the type displayed is Group.

opens the Display Properties Dialog Box (p. ), which allows you to change the color, visibility, and

other properties for the selected object.

Transform...

opens the Transformations Dialog Box (p. ), which allows you to translate, rotate, and scale the

selected object.

Iso-Value...

opens the Iso-Value Dialog Box (p. ), which allows you to change the isovalue of an isosurface.This

push button is available only if the geometric object selected in the Names list is an isosurface or an

object on an isosurface (contour on an isosurface, for example); otherwise it is grayed out.

Pathlines...

opens the Pathline Attributes Dialog Box (p. ), which allows you to set the maximum number of

steps for the selected pathlines.

Scene Composition

contains controls for enabling overlays and bounding frames.

Overlays

activates the superimposition of a new geometry onto a currently displayed geometry. See Advanced

Graphics Overlays (p. ) for details.

Draw Frame

activates the display of a bounding frame in the graphics display. See Adding a Bounding Frame (p. )

Frame Options...

opens the Bounding Frame Dialog Box (p. ), in which you can define properties of the bounding frame.

See Adding a Bounding Frame (p. ) for details.

Delete Geometry

deletes the geometric object that is currently selected in the Names list.The ability to delete individual

objects is especially useful if you have overlays on and you generate an unwanted object (for example,

if you generate contours of the wrong variable).You can simply delete the unwanted object and continue

your scene composition, instead of starting over from the beginning.

Apply

saves the status of Overlays and Draw Frame.When you turn Overlays or Draw Frame on or off, you

must click the Apply button to see the effect of the change on subsequent display operations.

To modify the color, visibility, and other display properties for individual geometric objects in the

graphics display, use the Display Properties dialog box. You can open this dialog box by clicking the

Display... push button in the Scene Description Dialog Box (p. ). See Changing an Object’s Display

Properties (p. ) for details about the items below.

Controls

Geometry Name

displays the name of the object you selected for modification in the Scene Description Dialog Box (p. ).

Visibility

contains check buttons that control options related to the visibility of the selected object. See Controlling

Visibility (p. ) for details.

Visible

toggles the visibility of the selected object. If it is turned on, the object will be visible in the display,

and if it is turned off, the object will be invisible.

Lighting

turns the effect of lighting for the selected object on or off.You can choose to have lighting affect

only certain objects instead of all of them. Note that if Lighting is turned on for an object such as a

contour or vector plot, the colors in the plot will not be exactly the same as those in the colormap at

the left of the display.

Faces

toggles the filled display of faces for the selected mesh or surface object.Turning Faces on has the

same effect as turning on the display of faces in the Mesh Display Dialog Box (p. ).

Outer Faces

toggles the display of outer faces.

Edges

toggles the display of interior and exterior edges of the geometric object.

Perimeter Edges

toggles the display of the outline of the geometric object. (This option has no effect on the display

of meshes.)

Feature Edges

toggles the display of feature lines (if any) of the geometric object.

Lines

toggles the display of the lines (if any) in the geometric object.

Nodes

toggles the display of the nodes (if any) in the geometric object.

Colors

contains controls for setting face, edge, line, and node colors, and transparency for faces. See Controlling

Object Color and Transparency (p. ) for details.

Color

specifies the face, edge, line, or node color for modification.When you turn on this button, the color

scales below will show the current color specification, which you can modify by moving the sliders

on the color scales.

Red, Green, Blue

are color scales with which you can specify the RGB components of the face, edge or line color.

sets the relative transparency of the selected object. An object with a transparency of  is opaque,

and an object with a transparency of  is transparent.

You can use the Transformations dialog box to translate, rotate, or scale individual objects in the

graphics display. To open this dialog box, click the Transform... push button in the Scene Description

Dialog Box (p. ). See Transforming Geometric Objects in a Scene (p. ) for details about the items

below.

Controls

Meridional

(3D only) enables the display of the meridional view.This option is especially useful in turbomachinery

applications.

Translate

Translate

contains X, Y, and Z real number fields in which you can enter the distance by which to translate the se-

lected object in each direction.

Rotate by

contains X, Y,and Z integer number fields in which you can enter the number of degrees by which to rotate

the selected object about each axis.

Rotate about

specifies the point about which to rotate the object.

Scale

contains X, Y, and Z real number fields in which you can enter the amount by which to scale the selected

object in each direction.To avoid distortion of the object’s shape, be sure to specify the same value for

The Iso-Value dialog box allows you to change the isovalue of an isosurface. The isosurface can be

selected directly in the Names list or indirectly by selecting an object displayed on the isosurface.

When you change the isovalue, any contours, vectors, and so on that were displayed on the original

isosurface will be displayed on the isosurface with the new isovalue. To open this dialog box, click the

Iso-Value... push button in the Scene Description Dialog Box (p. ). See Modifying Iso-Values (p. )

Controls

displays the name of the geometric object (isosurface) you selected for modification in the Scene Descrip-

tion Dialog Box (p. ).

Min, Max

show the minimum and maximum values of the isosurface variable.

Value

sets the new isovalue for isosurfaces. After you change the value and click Apply, contours, vectors, or

Min, Max

Value

pathlines that were displayed on the original isosurface will be displayed for the new isovalue.You can

also use the slide bar to change the Value.

The Pathline Attributes dialog box allows you to change the number of steps used in the computation

of pathlines. This is most useful in creating animations of pathlines. To open this dialog box, click the

Pathlines... button in the Scene Description Dialog Box (p. ). See Modifying Pathline Attributes (p. )

Controls

displays the name of the geometric object you selected for modification in the Scene Description Dialog

Box (p. ).

Max Steps

sets the new maximum number of steps for pathline computation. After you change the value and click

Apply, the selected pathline will be recomputed and redrawn.

The Bounding Frame dialog box allows you to add a bounding frame with optional measure markings

to the display of the domain. See Adding a Bounding Frame (p. ) for details about the items in this

Controls

Frame Extents

indicates the extents of the bounding frame.

Domain

specifies that the frame should encompass the domain extents.

Display

specifies that the frame should encompass the portion of the domain that is shown in the display.

Axes

contains controls for specifying the frame boundaries and measurements. See Adding a Bounding

Frame (p. ) for instructions on using these items.

Display

Axes

Display

updates the active graphics window with the current frame settings.

With the Views dialog box, you can make various modifications to the view displayed in the active

graphics window. See Modifying the View (p. ) for details about the items below.

Controls

Views

lists the currently defined views. Clicking on a view name highlights that name and enters it into the

Name field. Double-clicking on a view name restores that view in the active graphics window.

Save Name

specifies the name to use when saving a view.

Actions

contains buttons for performing various actions related to the Views list and the Save Name.

Default

restores the “front” view in the active graphics window.

Auto Scale

modifies the view in the active graphics window by scaling and centering the current scene without

changing its orientation.

Previous

allows you to return to previous displays.

Save

stores the view in the active graphics window with the name in the Save Name box. See Saving

Views (p. ) for details.

Delete

removes the selected view name from the Views list.

Important

Be careful not to delete any of the pre-defined views.

Read...

opens The Select File Dialog Box (p. ), in which you can specify the name of a view file to be read.

See Reading View Files (p. ) for details.

Write...

opens the Write Views Dialog Box (p. ), in which you can select the views to be saved to a view file.

See Saving Views (p. ) for details.

Mirror Planes

Write...

displays a list of all symmetry planes in the domain. Mirror images are drawn for all selected symmetry

planes. See Mirroring and Periodic Repeats (p. ) for details.

Define Plane...

opens the Mirror Planes Dialog Box (p. ), in which you can define a mirror plane for a non-symmetric

domain.

Periodic Repeats

indicates the number of periodic repetitions to be displayed. See Mirroring and Periodic Repeats (p. )

Define...

opens the Graphics Periodicity Dialog Box (p. ), in which you can define periodicity for a periodic

domain.

Camera...

opens the Camera Parameters Dialog Box (p. ).

The Write Views dialog box allows you to save selected views to a view file. To open it, click Write...

in the Views Dialog Box (p. ). This feature allows you to transfer views between case files. See Saving

Controls

Views to Write

is a selectable list of the defined views.The selected views will be saved to a view file when you click OK.

The Mirror Planes dialog box allows you to define a symmetry plane for a non-symmetric domain for

use with graphics. To open it, click Define Plane... in the Views Dialog Box (p. ). See Mirroring for

Graphics (p. ) for details.

Controls

Plane Equation

contains inputs for specifying the equation for the mirror plane: A X + B Y+ C Z = Distance.

contains a list of all mirror planes you have defined using this dialog box. (Mirror planes that exist in the

domain due to symmetry will not appear in this list, since they cannot be modified.)

Add

Add

adds the plane defined by the Plane Equation to the Mirror Planes list.

Delete

deletes the plane(s) selected in the Mirror Planes list.

The Graphics Periodicity dialog box allows you to define a periodic repeats, periodic rotation or

translation for a non-periodic domain for use with graphics. To open it, click Define... under Periodic

Repeats in the Views Dialog Box (p. ). See Periodic Repeats for Graphics (p. ) for details.

Controls

Cell Zones

contains the list of the zones in the mesh.You can select one or more zones in this list and specify different

periodicity parameters for each zone separately.

Associated Surfaces

contains the list of the surfaces associated with the selected cell zone.

specifies Rotational or Translational periodicity.

Angle

specifies the angle by which the domain is rotated to create the periodic repeat.This item is available

when you select Rotational as the Periodic Type.

specifies the distance in the X, Y, and Z directions by which the domain is translated to create the periodic

repeat.This item will appear when you select Translational as the Periodic Type.

specifies the direction vector (X,Y,Z) for the axis of rotation.This item is available when you select Rota-

tional as the Periodic Type and the domain is three-dimensional.

specifies the origin of the axis of rotation.This item is available when you select Rotational as the Peri-

odic Type.

Number of Repeats

specifies the number of times you want to repeat the periodic domain.

Set

applies the periodicity you have defined for the case setup.

odic Type.

Set

Reset

removes any periodicity you have defined, and returns to the default periodicity for the domain (no

periodicity for a non-periodic domain).

The Camera Parameters dialog box allows you to modify the “camera” through which you are viewing

the graphics display. See Controlling Perspective and Camera Parameters (p. ) for details about the

Controls

Camera

contains a drop-down list of the parameters that define the camera (Position, Target, Up Vector, and

Field) and X, Y, and Z fields in which you can define the coordinates or field distances for the parameter

selected in the drop-down list. Figure . : Camera Definition (p. ) illustrates the definition of the

camera by these parameters.

contains a drop-down list that allows you to select a Perspective or Orthographic view.

(Dial and Sliders)

allow you to rotate and scale the graphics display.The slider on the scale to the left of the dial rotates

the display about the horizontal axis at the center of the screen, the slider on the scale below the dial

rotates the display about the vertical axis at the center of the screen, and the dial controls rotation about

the axis at the center of and perpendicular to the screen.The slider on the scale to the right of the dial

zooms in or out in the display. See Rotating the Display (p. ) and Zooming the Display (p. ) for details.

Important

When you are using the sliders and dial to manipulate the view, you may want to turn

off Wireframe Animation in the Display Options Dialog Box (p. ), so that you can

Important

watch the display move interactively while you are moving the slider or the dial indic-

ator.

The Lights dialog box provides an interactive mechanism for placing colored, directional lights in a

scene. See Adding Lights (p. ) for details about the items below.

Controls

Light ID

indicates the light that is being added, deleted, or modified. By default, light  is defined to be dark gray

with a direction of (,,).

Light On

indicates whether or not the light specified in Light ID is on or off. By turning off the Light On option for

a particular light, you can remove this light from the display, while still retaining its definition.To add it

to the display again, simply turn on the Light On button.

Direction

allows you to specify the direction of the light (the position on the unit sphere from which the light em-

anates) by entering the X, Y, and Z coordinates or by computing the coordinates based on the current

view in the graphics window.

X,Y,Z

specify the direction of the light. For example, the direction (,,) means that the rays from the light

will be parallel to the vector from (,,) to the origin.

Use View Vector

updates the X,Y,Z fields with the appropriate values for the current view in the active graphics window,

and shines a light in that direction. Instead of entering the X,Y,Z values for a light’s direction vector,

you can use your mouse to change the view in the graphics window so that your position in reference

to the geometry is the position from which you would like a light to shine.You can then click the Use

View Vector button to update the X,Y,Z fields with the appropriate values for your current position

and update the graphics display with the new light direction.This method is convenient if you know

where you want a light to be, but you are not sure of the exact direction vector.

Color

allows you to specify the light color with sliders.You can create your desired color by increasing and de-

creasing the slider values for the colors Red, Green, and Blue.You can also enter a descriptive string (for

example, lavender) in the Color field.

Active Lights

shows the position and color of all defined directional lights, and allows you to change the position of a

light. All directional lights in ANSYS Fluent are assumed to be at infinity and pass through the unit sphere

at the position shown. All light rays arriving at the scene from one light are parallel.The colored markers

on the surface of the sphere represent the color and direction of these distant lights.These lights point

towards the center of the sphere (the origin, which is usually where the geometry is).

Lighting Method

specifies the method to be used in lighting interpolation: Off, Flat, Gouraud, or Phong. (Flat is the most

basic method: there is no interpolation within the individual polygonal facets. Gouraud and Phong have

smoother gradations of color because they interpolate on each facet.) When Off is selected, lighting effects

are disabled.

Headlight On

enables constant lighting effects in the direction of the view.

Reset

Reset

resets the light definitions to their last saved state (the lighting that was in effect the last time you opened

the dialog box or clicked on Apply).

The Colormap dialog box allows you to select and modify existing colormaps. See Selecting a

Colormap (p. ) for details.

Controls

Show Colormap

this option is only visible when accessed through a graphics object dialog box, such as Contours or

Vectors. It allows you to turn the display of the colormap in the graphics window on/off.

Labels

allows you to customize the display of your colormap labels.

Show All

Enable this option if you want all the labels to show alongside the colormap. Disable if you want to

skip some of the label displays.

Skip

sets the number of labels to be skipped.

Number Format

contains controls for changing the format of the labels on the color scale.These labels are the char-

acter strings used to define the color divisions at the left of the graphics window.

Type

sets the form of the labels.You may select from a drop-down list of options, including the following:

general

displays the real value with either float or exponential form based on the size of the number

and the defined Precision.

float

displays the real value with an integral and fractional part (for example, . ), where the

number of digits in the fractional part is determined by Precision.

exponential

displays the real value with a mantissa and exponent (for example, .0e-), where the number

of digits in the fractional part of the mantissa is determined by Precision.

Precision

Precision

defines the number of fractional digits displayed in the labels.

Colormap

contains controls for the colormap size and scale, and for selection of a defined colormap.

Log Scale

enables the use of a logarithmic scale for the color scale (rather than the default decimal scale). See

Specifying the Colormap Size and Scale (p. ) for details.

Colormap Size

specifies the number of distinct colors in the colormap.You may specify from  to  colors.

Currently Defined

contains a drop-down list of all pre-defined colormaps and all custom colormaps defined by you.

Select the colormap to be used from this list.

Edit...

opens the Colormap Editor Dialog Box (p. ), in which you can create a custom colormap.

The Colormap Editor dialog box allows you to create custom colormaps. See Creating a Customized

Colormap (p. ) for details about the items below.

Controls

(The Drawing Area)

is used to interactively modify colormaps.You can use the notion of anchor points to interpolate linearly

between two defined anchor points.The colors at the top of the dialog box allow you to preview the

colormap that is being defined.The black bar and white squares below the colors allow you to set, delete,

and modify anchor points.

Color

specifies color components for the currently selected anchor point.

Color Space

gives you a choice of selecting the color specification.

RGB

enables the specification of colors based on their red, green, and blue components.

HSV

enables the specification of colors based on their hue, saturation, and value.

RGB

HSV

are scales with which you can specify the RGB components of the selected anchor color.These

scales will appear when RGB is selected.

Hue, Saturation,Value

are scales with which you can specify the HSV components of the selected anchor color.These

scales will appear when HSV is selected.

Colormap

lists colormap names and the name of the colormap being edited.

Name

sets the name of the colormap being edited/selected.You can rename existing colormaps and provide

names for new colormaps.

contains a drop-down list of all pre-defined colormaps and all custom colormaps defined by you.You

can select a colormap to be modified from this list.

You can use the Annotate dialog box to add text with optional attachment lines to the graphics

windows, or to modify existing text. See Adding Text Using the Annotate Dialog Box (p. ) for details

Controls

Names

contains a selectable list of all annotation text strings that have been defined.You can choose a text string

to be deleted or edited.

Delete Text

deletes the text strings selected in the Names list from the display.

Annotation Text

contains the annotation text string you want to add, or the annotation text string for the item selected

in the Names list.

Font Specification

contains controls for defining or modifying the font in the annotation text string.

Name

contains a drop-down list of various font styles.

Weight

Name

Weight

contains a drop-down list from which you can select Medium or Bold.

Color

contains a drop-down list of colors that can be used for the text.

Slant

contains a drop-down list from which you can select Regular or Italic as the slant type.

Size

contains a drop-down list of font sizes (in points).

Add

adds the current Annotation Text to the active graphics window. A dialog box will prompt you to select

a screen location using the mouse-probe button on your mouse (see Controlling the Mouse Button

Functions (p. ) for more information on setting the mouse buttons).

Edit

updates the edited text in the active graphics window.This button will replace the Add button when you

are editing an existing text string from the Names list.

Clear

removes all annotation text and attachment lines from the active graphics window.

The Plots task page allows you to create plots (XY, histograms, profiles, and so on) of your computa-

tional results. See Displaying Graphics (p. ) for more information.

Controls

Plots

contains a listing of the various plot types available in ANSYS Fluent.

You can double-click an item in the Plots list to open the corresponding dialog box, or you can

XY Plot

selecting this item and clicking the Set Up... button opens the Solution XY Plot Dialog Box (p. ).

Histogram

selecting this item and clicking the Set Up... button opens the Histogram Dialog Box (p. ).

File

Histogram

File

selecting this item and clicking the Set Up... button opens the File XY Plot Dialog Box (p. ).

Profiles

two types of profile plots are available:

Profile Data

selecting this item and clicking the Set Up... button opens the Plot Profile Data Dialog Box (p. ).

Interpolated Data

selecting this item and clicking the Set Up... button opens the Plot Interpolated Data Dialog

Box (p. ).

FFT

selecting this item and clicking the Set Up... button opens the Fourier Transform Dialog Box (p. ).

Set Up...

displays the dialog box corresponding to the selected item in the Plots list.

... Solution XY Plot Dialog Box

... Histogram Dialog Box

... File XY Plot Dialog Box

... Plot Profile Data Dialog Box

... Plot Interpolated Data Dialog Box

... Fourier Transform Dialog Box

... Plot/Modify Input Signal Dialog Box

... Axes Dialog Box

... Curves Dialog Box

The Solution XY Plot dialog box allows you to display zone, surface and file data in an XY plot format.

See Steps for Generating Solution XY Plots (p. ) for details about the items below.

You can also access the Solution XY Plot dialog box through the Postprocessing ribbon tab.

Postprocessing → Plots → XY Plot → New...

Plots Task Page

Controls

XY Plot Name

is the name for a solution XY plot definition.You can specify a name or use the default name  xy-

plot-id.This control appears only for solution XY plot definitions.

Options

contains check buttons that control the presentation of node or cell-averaged values, the selection of

Options

axis functions, and the ability to write the plot data to a file.

Node Values

toggles the node averaging of the data presented in the plot. If the option is inactive, cell values are

presented. See Choosing Node or Cell Values (p. ) for details.

Position on X Axis, Position on Y Axis

set the -axis or -axis function to be the position. If one of these options is turned on, the other will

automatically be turned off.You can turn both options off to generate a plot of one flow-field function

vs. another, selecting the function for each axis using the X Axis Function and Y Axis Function drop-

down lists.

Write to File

activates the file-writing option.When this option is selected, the Plot push button will change to

Write.... Clicking on the Write... button will open the Select File dialog box (The Select File Dialog

Box (p. ) and The Select File Dialog Box (Windows) (p. )), in which you can specify a name and

save a file containing the plot data.The format of this file is described in XY Plot File Format (p. ).

Order Points

specifies that plot data being saved to a file should be sorted in order of ascending  axis value.This

option is available only when the Write to File option is turned on.

Plot Direction

contains inputs for defining the plot direction.

If Direction Vector (the default) is selected in the X Axis Function or Y Axis Function drop-down

list (whichever is the position axis), the inputs are the components of the direction vector. The

position axis of the plot will have coordinate values that correspond to the dot product of the data

coordinate vector with the plot direction vector. See Steps for Generating Solution XY Plots (p. )

X

is the component in the  direction.

Y

Z

If Curve Length is selected in the X Axis Function or Y Axis Function drop-down list (whichever

is the position axis), the inputs are the direction along the length of the surface selected in the

Surfaces list. See Steps for Generating Solution XY Plots (p. ) for details.

Default

specifies the plot direction as the direction of increasing curve length.

Reverse

specifies the plot direction as the direction of decreasing curve length.

Show

displays the selected surface in the graphics window, marking the start of the surface with a blue dot

and the end of the surface with a red dot. ANSYS Fluent will also display arrows on the surface

showing the direction in which the variable will be plotted.

Y Axis Function, X Axis Function

contain lists of solution variables that can be used for the  or  axis of the plot. If the Position on X

Axis option is turned on, X Axis Function will become a single drop-down list, containing two options:

Direction Vector (to plot the selected variable as a function of position along a specified direction vector)

and Curve Length (to plot the selected variable as a function of position along the length of a specified

curvilinear surface). See Steps for Generating Solution XY Plots (p. ) for details.

Likewise, if Position on Y Axis is turned on, Y Axis Function will become a single drop-down list

containing Direction Vector and Curve Length. If both Position on X Axis and Position on Y

Axis are turned off, you can select field functions for both axes using the X Axis Function and Y

Axis Function lists.

Note

When running the parallel version of ANSYS Fluent, Curve Length is only supported when

the curvilinear surface is contained within a single partition.

File Data

is a selectable list of the plot titles associated with the loaded external data files.You may choose any

number of files for the data plot.The files are loaded using the Load File... push button.The format of

these files is presented in XY Plot File Format (p. ). See Including External Data in the Solution XY

Plot (p. ) for details.

Load File...

opens the Select File dialog box (The Select File Dialog Box (p. )), in which you can select the plot file

to be read. See Including External Data in the Solution XY Plot (p. ) for details. After the external file is

loaded, its plot title will be displayed in the File Data list.

Free Data

removes the files selected in the File Data list.

Surfaces

is a selectable list of surfaces in the solution domain.You may choose any number of surfaces for the data

plot.

Point

Line/Rake

Plane

Quadric

Point

Line/Rake

Plane

Quadric

Iso-Clip

Plot

plots the specified surface and/or file data in the active graphics window using the current axis and curve

attributes. If the Write to File option is turned on, this button becomes the Write... button.

Write...

opens the Select File dialog box (The Select File Dialog Box (p. )), in which you can save the plot data

to a file.This button replaces the Plot button when the Write to File option is turned on.

Axes...

opens the Axes Dialog Box (p. ), which allows you to customize the plot axes.

Curves...

opens the Curves Dialog Box (p. ), which allows you to customize the curves used in the XY plot.

Save/Plot

attributes and saves the XY plot definition.This button appears only for solution XY plot definitions and

replaces the Plot button.

The Histogram dialog box allows you to create histograms of selected geometric or physical data. See

Steps for Generating Histogram Plots (p. ) for details about the items below.

Controls

Options

contains the check buttons for current histogram options.

Auto Range

toggles the ability to specify the minimum and maximum range of scalar values in the histogram

print or plot. If the option is not active, the Min and Max fields are editable, and you may specify the

desired range. If the option is active, the range is defined by the minimum and maximum values in

the computational domain.

Global Range

toggles the ability to specify the minimum and maximum values on the range of values on the selected

surfaces, rather than in the entire domain.

Divisions

sets the number of data intervals that will exist in the histogram.

Zone Types

contains a list of available face or cell zone types.

Axes...

Curves...

opens the Curves Dialog Box (p. ), which allows you to customize the curves used in the histogram

plot.

Histogram of

contains a list of scalar quantities that can be used in the histogram.

Min

displays or allows definition of the minimum value of the selected scalar quantity used in the histogram.

Max

displays or allows definition of the maximum value of the selected scalar quantity used in the histogram.

Zones

contains a list of available face or cell zones.

Print

displays the histogram interval.

Plot

displays a plot of the percentage of the total number of cells versus the scalar quantity in the active

Compute

computes the minimum and maximum cell values of the selected scalar quantity.The values are displayed

in Min and Max.

The File XY Plot dialog box allows you to display data read from one or more files in an abscissa/or-

dinate plot form. The format of the plot file is described in XY Plot File Format (p. ). See Steps for

Generating XY Plots of Data in External Files (p. ) for details about the items below.

Controls

Files

Controls

Files

contains operations and information related to the loaded files.

Load...

opens the Select File dialog box, where you can select the file(s) you want to plot.

Remove

removes the selected file from the File Names list.This also removes any curves associated with that

file.

File Names

lists the files that you have loaded.

Data Sets

lists the available data sets for files (typically .xy) that contain two columns monitoring the same

value at different locations.You can select which data sets you want to plot by selecting/de-selecting

the listed items.

Variables

lists X and Y variables for the selected file.

X Axis Variable

lists the variables that you can select for the X axis.The highlighted X variable will be added to the

Curve Information list in coordination with the selected Y Axis Variables. Changing the selected X

Axis Variable updates all the related curves shown in the Curve Information list.

Y Axis Variables

lists the variables that you can select for the Y axis.The highlighted Y variables will be added to the

Curve Information list in coordination with the selected X Axis Variable. Changing the selected Y

Axis Variables updates how many curves are shown in the Curve Information list.

Curves

lists what items will be plotted and how they will be labeled in the legend.

Curve Information

lists the curves that will be plotted. Information about each curve is shown in the following order:

. The name of the file where the data originated.

. [ column file (typically .xy) only] The location on the model where the data originated.

. X Variable.

. Y Variable.

Legend Names

lists the name for each curve that will be listed in the legend when the plot is displayed in the

graphics window. (see Change Legend Entry to learn how to change the legend name for a curve).

Remove

removes the selected curve from the Curve Information list.

Change Legend Entry

allows you to change the name that will appear in the plot legend in the graphics window for a par-

ticular curve.To use:

Plot

contains text entry boxes for the various plot labels.

Title

lets you enter a title for the plot.

Legend Label

lets you enter a title for the legend.

X Axis Label

lets you label the X axis.

Y Axis Label

lets you label the Y axis.

Plot

click Plot to plot the data listed in the Curve Information list.

Axes...

Curves...

The Plot Profile Data dialog box allows you to display an XY plot of the original data points of a

boundary profile before it is interpolated onto the cell faces of a boundary. See Steps for Generating

Plots of Profile Data (p. ) for details about the items below.

Controls

Profile

under Y Axis Function.

Y Axis Function

Controls

Profile

contains a selectable list of the fields available in the selected profile that can be used for the  axis of

the plot.

X Axis Function

contains a selectable list of the variables that can be used for the  axis of the plot.

Plot

displays an XY plot of the data points from the selected profile.

Axes...

Curves...

The Plot Interpolated Data dialog box allows you to display an XY plot of the values assigned to the

cell faces when a profile file has been interpolated on a boundary. See Steps for Generating Plots of

Interpolated Profile Data (p. ) for details about the items below.

Controls

Zones

contains a selectable list of the zones for which a profile field has been set as one or more of the parameters

are displayed under Y Axis Function.

contains a selectable list of the profile-related parameters in the selected zone that can be used for the

axis of the plot.The name of the parameter will be the same as that of the drop-down list in the

boundary condition dialog box from which the profile field was selected.

contains a selectable list of the geometry variables that can be used for the  axis of the plot.

Plot

displays an XY plot of the cell face values (as interpolated from the data points of the profile file) of the

selected zone.

Axes...

Axes...

Curves...

The Fourier Transform dialog box allows you to analyze your time dependent data using the Fast

Fourier Transform (FFT) algorithm. See Fast Fourier Transform (FFT) Postprocessing (p. ) for details

Controls

Options

lets you write the FFT data to a file or display the FFT data in a graphics window.

Write FFT to File

allows you to write out the FFT data directly to a file.When selected, the Plot FFT... buttons becomes

the Write FFT... button.

Acoustics Analysis

enables the acoustics-relevant spectrum options (sound pressure level spectra and frequency band

charts), and specifies that the overall sound pressure level is calculated and displayed in the console

when you plot or write the FFT data. All dB-measured quantities are based on the Reference Acoustic

Pressure.

Process Options

contains options to analyze signal data.

Process Receiver

allows you to analyze receiver data stored in memory.

Process File Data

allows you to analyze signal data from an existing input file.

contains a list from which you can select the function for the  axis.

Receiver

contains a list of receivers from which you can select when the Process Receiver option is enabled.

Plot/Modify Input Signal...

opens the Plot/Modify Input Signal Dialog Box (p. ), which you can use to plot the input signal, as well

as customize the data set and define spectrum smoothing in preparation for applying the FFT algorithm.

allows you to specify the reference acoustic pressure (for example,

in Equation . (p. )) used to

calculate the dB-measured quantities when the Acoustics Analysis option is enabled.

Plot Title

lets you create a new title or edit the original title for the FFT plot. By default, ANSYS Fluent adds the

string “Spectral Analysis of” to the title originally applied to the input signal plot.

allows you to create a new  axis label or edit the original  axis label. By default, the Y Axis Label cor-

responds to the selection in the Y Axis Function drop-down list.

allows you to create a new  axis label or edit the original  axis label. By default, the X Axis Label corres-

ponds to the selection in the X Axis Function drop-down list.

Y Axis Variable

if your input report file contains multiple report definitions, this allows you to specify the  axis variable.

Files

lists the loaded input signal data files.

Load Input File...

loads an input signal data file into ANSYS Fluent for FFT analysis.The input file is listed under Files.

Free File Data

removes data from FFT analysis once the input signal data file is selected in the Files list.

Plot FFT

displays the FFT data in a graphic window and, if Acoustics Analysis is enabled, calculates the overall

Plot FFT

sound pressure level in dB (based on the Reference Acoustic Pressure) and displays it in the console. If

the Write FFT to File option is selected, then this button becomes the Write FFT button, which opens

a file selection dialog box so that you write the FFT data to a file.

Write FFT

opens The Select File Dialog Box (p. ) in which you can specify a name and save the FFT data to a file.

If Acoustics Analysis is enabled, the overall sound pressure level will be calculated in dB (based on the

Reference Acoustic Pressure) and displayed in the console at this time. If the Write FFT to File option

is selected, then the Plot FFT button changes to the Write FFT button.

Axes...

Curves...

opens the Curves Dialog Box (p. ), which allows you to customize the curves used in the plot.

The Plot/Modify Input Signal dialog box allows you to plot the input signal, as well as customize the

data set and define spectrum smoothing in preparation for applying the FFT algorithm. It is opened

from the Fourier Transform Dialog Box (p. ). See Using the FFT Utility (p. ) for details about the

Controls

Options

allows you to process some or all of the input signal data.

Clip to Range

allows you to analyze a portion of the input signal by specifying data range.

Subtract Mean Value

reduces y axis quantities by the mean value of the relevant signal property.

Subdivide into Segments

enables / disables spectrum smoothing, which can suppress spurious amplitude fluctuations in the

Fourier spectrum by splitting the input signal into multiple overlapping segments, so that ANSYS

Fluent can apply the FFT algorithm on each segment and then average the resulting spectra.The

spectrum smoothing is controlled by the settings in the Segment Control group box. See Customizing

the Input and Defining the Spectrum Smoothing (p. ) for further details.

Signal Statistics

displays signal information.

Min

displays the minimum value for the input signal.

Max

displays the maximum value for the input signal.

Mean

displays the average value for the input signal.

Variance

displays the variance for the input signal.

displays the total number of samples in the input signal data set.

Min Frequency

displays the finest possible frequency resolution for the input signal.

X Axis Range

allows for a portion of the input signal to be analyzed when the Process the whole data option is turned

off.

Min

specifies a minimum value for the  axis.

Max

specifies a maximum value for the  axis.

Set Defaults

resets the  axis minimum and maximum values to their original value and turns on the Process the

whole data option.

Signal Plot Title

lets you create a new title or edit the original title for the input signal plot. By default, the Signal Plot

Title corresponds with the title originally applied to the input signal plot.

responds with the  axis label originally applied to the input signal plot.

ponds with the  axis label originally applied to the input signal plot.

Window

lets you specify a windowing technique to remove discontinuities in the FFT calculation.

None

applies no windowing technique.This is the default setting.

Hamming

applies the Hamming technique.

Hanning

applies the Hanning technique.

Barlett

applies the Barlett technique.

Blackman

applies the Blackman technique.

Segment Control

provides settings that control the spectrum smoothing when Subdivide into Segments is enabled.

Control Method

allows you to specify how you want to define the segment size from the following:

Samples

bases the segment size on the Samples per Segment.

Frequency

bases the segment size on the Frequency Resolution

in Hertz units.

Samples per Segment

defines the number of samples in each segment when Samples is selected from the Control Method

list.

Frequency Resolution

defines the desired frequency resolution

in Hertz units when Frequency is selected from the

Control Method list.

Overlap

ranges from  to  and defines how much adjacent segments overlap.This setting is applicable re-

gardless of which Control Method you select.

Apply/Plot

Overlap

applies any changes you have made in the dialog box and displays the input signal data in a graphics

window.

Axes...

Write...

opens The Select File Dialog Box (p. ), in which you can save the signals to a file.

The Axes dialog box allows you to independently control the characteristics of the ordinate and abscissa

on an XY plot or histogram. You can change the labels, scale, range, number format, and major and

minor rules visibility and appearance. Note that the title following Axes in the dialog box indicates

which plot environment you are changing. You can set different parameters for each type of plot that

ANSYS Fluent can generate. See Using the Axes Dialog Box (p. ) for details about the items below.

Controls

Axis

contains check buttons that allow you to set abscissa ( -axis) or ordinate ( -axis) characteristics.

X

allows you to specify the abscissa characteristics.

Y

allows you to specify the ordinate characteristics.

Label

defines the character string that will label  the active axis (the one selected in Axis) in the display.

Options

contains check buttons that (de)activate scale, range, major rules, and minor rules.

Log

toggles logarithmic scaling of the active axis. By default, decimal scaling is used.

Auto Range

toggles automatic computation of the range of the active axis. If you deactivate this option, you may

input the Minimum and Maximum values in the Range box.

Major Rules

Auto Range

toggles the display of major rules on the active axis. Major rules are the horizontal or vertical lines

that mark the primary data divisions and span the whole plot window to produce a “grid.”

Minor Rules

toggles the display of minor rules on the active axis. Minor rules are the horizontal or vertical lines

that mark the secondary data divisions and span the whole plot window to produce a “grid.”

contains controls for changing the format of the data labels on the active axis. Data labels are the character

strings used to define the primary data divisions on the axes.

Type

sets the form of the data labels.You may select from a drop-down list of options, including the follow-

ing:

general

displays the real value with either float or exponential form based on the size of the number and

the defined Precision.

float

displays the real value with an integral and fractional part (for example, . ), where the number

of digits in the fractional part is determined by Precision.

Precision

defines the number of fractional digits displayed in the data labels.

Range

contains the range or extents of the active axis.To set the range manually, you must turn off Auto Range.

Otherwise the extents are computed automatically.

Minimum

sets the minimum data value for the active axis.

Maximum

sets the maximum data value for the active axis.

Minimum

Maximum

contains controls for modifying the appearance of the major rules.To use these controls you must activate

Major Rules in the Options list.

Color

sets the color of the major rules from a drop-down list with numerous color selections.

Weight

sets the line thickness of the major rule. A line of weight . is normally  pixel wide. A weight of .

would make the line twice as thick ( pixels wide).

contains controls for modifying the appearance of the minor rules.To use these controls you must activate

Minor Rules in the Options list.

Color

sets the color  of the minor rules from a drop-down list with numerous color selections.

Weight

sets the line thickness of the minor rule. A line of weight . is  pixel wide. A weight of . would

make the line twice as thick ( pixels wide).

The Curves dialog box allows you to modify the appearance of the lines and markers used in XY plots.

changing. You can set different parameters for each type of plot that ANSYS Fluent can generate. See

Using the Curves Dialog Box (p. ) for details about the items below.

Controls

Curve #

defines the active curve number.The present and future marker and line styles apply to the defined curve

number.The curves are numbered sequentially, starting from . For example, if you were plotting flow-

field values on two zones, the first zone would be curve , and the second, curve . If the plot contains

only one curve, the Curve # is set to  and is not editable.

Sample

Sample

displays a single marker and line with the current style attributes.

Line Style

contains controls for modifying the appearance of the active curve.

Pattern

sets the pattern of the active curve. A drop-down list allows you to set the line pattern. Except for

center and phantom lines, the list displays examples of the pattern choices. A center line alternates

a very long dash and a short dash and a phantom line alternates a very long dash and a double short

dash.

Color

sets the color of the active curve. A drop-down list allows you to select from a list of color names.

Weight

sets the thickness of the active curve. A line weight of . is normally  pixel wide.Therefore, a weight

of . would make the line twice as thick ( pixels wide).

Marker Style

contains controls for modifying the appearance of the active curve’s marker.

Symbol

sets the symbol used to mark data.You can select the symbol from a drop-down list that contains all

the symbol choices.The Sample box will allow you to experiment with various markers. For example,

in plotting pressure-coefficient data on the upper and lower surfaces of an airfoil, the symbol /*\

(filled-in upward-pointing triangle) could be used for the marker representing the upper surface data,

and the symbol \*/ (filled-in downward-pointing triangle) could be used for the marker representing

the lower surface data.

Color

sets the color of the marker on the active line number. A drop-down list allows you to select from a

list of color names.

Size

Color

Size

sets the size of the data marker. A symbol of size . is .% of the height of the display screen, except

for the “.” symbol, which is always one pixel.

The Reports task page allows you to set up reports for your CFD simulation. Reports can be compiled

for fluxes, forces, projected areas, surface and volume integrals, among others. See Reporting Alphanu-

meric Data (p. ) for more information.

Controls

Reports

displays a list of available report types in ANSYS Fluent.

Reports Task Page

You can double-click an item in the Reports list to open the corresponding dialog box, or you can

Fluxes

selecting this item and clicking the Set Up... button opens the Flux Reports Dialog Box (p. ).

Forces

selecting this item and clicking the Set Up... button opens the Force Reports Dialog Box (p. ).

Projected Areas

selecting this item and clicking the Set Up... button opens the Projected Surface Areas Dialog Box (p. ).

Surface Integrals

selecting this item and clicking the Set Up... button opens the Surface Integrals Dialog Box (p. ).

Volume Integrals

selecting this item and clicking the Set Up... button opens the Volume Integrals Dialog Box (p. ).

allows you to report on one of the following three report types:

Sample

selecting this item and clicking the Set Up... button opens the Sample Trajectories Dialog Box (p. ).

Histogram

selecting this item and clicking the Set Up... button opens the Trajectory Sample Histograms Dialog

Box (p. ).

Summary

Histogram

Box (p. ).

Summary

selecting this item and clicking the Set Up... button opens the Particle Summary Dialog Box (p. ).

selecting this item and clicking the Set Up... button opens the Heat Exchanger Report Dialog Box (p. ).

Set Up...

opens the dialog box corresponding to the selected item in the Reports list.

... Flux Reports Dialog Box

... Force Reports Dialog Box

... Projected Surface Areas Dialog Box

... Surface Integrals Dialog Box

...Volume Integrals Dialog Box

... Sample Trajectories Dialog Box

...Trajectory Sample Histograms Dialog Box

... Particle Summary Dialog Box

... Heat Exchanger Report Dialog Box

... Parameters Dialog Box

... Use Input Parameter in Scheme Procedure Dialog Box

... Use Input Parameter for UDF Dialog Box

... Rename Dialog Box

... Parameter Expression Dialog Box

... Save Output Parameter Dialog Box

The Flux Reports dialog box allows you to compute the mass flow rate, heat transfer rate, and radiation

heat transfer rate on selected boundary zones. See Fluxes Through Boundaries (p. ) for details.

Controls

Options

contains the following option buttons:

turns on the computation of the mass flow rate for the selected boundary zones.

turns on the computation of the total heat transfer rate for the selected boundary zones.

turns on the computation of the total sensible heat transfer rate for the selected boundary zones. It

reports the total energy flux as defined in Equation . in the Theory Guide.

turns on the computation of the radiation heat transfer rate for the selected boundary zones.

(available only when the Eulerian wall film model is enabled) turns on the computation of the mass

flow rate for the selected boundary zone(s).

(available only when the Eulerian wall film model is enabled) turns on the computation of the film

heat transfer rate for the selected boundary zone(s).

Save Output Parameter...

opens the Save Output Parameter Dialog Box (p. ).

Boundaries

contains a selectable list of valid boundary zones for flux reporting.

Results

displays the results of the selected flux computation for each boundary zone selected.The summation

of the individual zone flux results is displayed in the box below the Results list.

Compute

computes the flux for each of the selected boundary zones and updates Net Results (for example, in

kg/s,W, and so on) and other reports, for example, Heat of Reaction Source.

Write...

opens the Select File dialog box (The Select File Dialog Box (p. ) and The Select File Dialog Box (Win-

dows) (p. )), which you can use to save the reported values to a file.

The Force Reports dialog box allows you to compute the forces along a specified vector, moments

about a specified center, and the coordinates of the center of pressure for selected wall zones. See

Forces on Boundaries (p. ) for details.

Controls

Options

Controls

Options

contains option buttons that control computation of the forces, moments, or center of pressure.

Forces

enables the computation of the pressure and viscous forces.

Moments

enables the computation of the pressure and viscous moments.

Center of Presure

enables the computation of the average location of the pressure.

contains the components of the force vector.This label is visible when the Forces option button is active.

X,Y,Z

are the components of the force vector along which the forces will be computed.

Moment Center

contains the Cartesian coordinates of the moment center.This label is visible when the Moments option

button is active.

X,Y,Z

are the Cartesian coordinates of the moment center about which moments will be computed.

Moment Axis

contains the Cartesian coordinates of the moment axis.This label is visible when the Moments option

X,Y,Z

are the Cartesian coordinates of the moment axis about which moments will be computed.

Coordinate

contains the value of the Cartesian coordinate that is fixed.This label is visible when the Center of Pressure

option button is active.

X,Y,Z

are the Cartesian coordinates, one of which will be fixed.

Value (n)

is the point where the selected Cartesian coordinate will be fixed.

Wall Zones

contains a selectable list of wall zones.The force or moment information is printed for each zone, and

then a total force or moment for all the zones is presented.

Print

Print

displays (in the console) the pressure, viscous (if appropriate), and total forces or moments, and the

pressure, viscous, and total force coefficients along the specified force vector or moment center for the

selected wall zones.The center of pressure coordinates will print to the console when the Center of

Pressure option is activated.

Write...

opens The Select File Dialog Box (p. ), which you can use to save the reported values to a file.

The Projected Surface Areas dialog box allows you to compute an estimated area of the projection

of selected surfaces along the ,

, or  axis. See Projected Surface Area Calculations (p. ) for details.

Controls

Projection Direction

indicates the direction along which to project the surface.

Min Feature Size

specifies the length of the smallest feature in the geometry that you want to resolve in the area calculation.

Area

displays the computed projected area.

Surfaces

contains a list of existing surfaces.You can select the surface(s) for which the projected area is to be cal-

culated in this list.

Compute

computes the area of the selected surfaces projected along the selected direction.The area will be printed

in the Area box and in the console window.

The Surface Integrals dialog box allows you to compute the area, mass and volume flow rate, standard

deviation, integral, flow rate, area-weighted average, custom vector-based flux, custom vector flux,

custom vector-weighted average, mass-weighted average, sum, facet average, facet minimum/maximum,

uniformity index (weighted by area or mass), vertex average, or vertex minimum/maximum quantity

of a specified field variable on a selected list of surfaces. See Surface Integration (p. ) for details.

Controls

Report Type

contains drop-down list that has options that control the method of surface integration.

Area

turns on the computation of the surface area.

turns on the computation of the area-weighted average on the surface(s).

Custom Vector Based Flux

turns on the computation of the vector-based flow rate of a quantity through the surface(s).

Custom Vector Flux

turns on the computation of the flow rate on a vector through the surface(s).

Custom Vector Weighted Average

turns on the computation of vector-weighted average of a quantity on the surface(s).

turns on the computation of the facet-averaged quantity on the surface(s).

turns on the computation of the facet minimum of a quantity on the surface(s).

turns on the computation of the facet maximum of a quantity on the surface(s).

Flow Rate

turns on the computation of the flow rate through the surface(s).

Integral

turns on the computation of the integral on the surface(s).

turns on the computation of the mass flow rate through the surface(s).

turns on the computation of the mass-averaged quantity on the surface(s).

turns on the computation of the standard deviation of a specified field variable on a surface.

Sum

turns on the computation of the summed quantity on the surface(s).

Uniformity Index - Mass Weighted

Sum

turns on the computation of the mass-weighted uniformity index of a quantity on the surface(s).

Uniformity Index - Area Weighted

turns on the computation of the area-weighted uniformity index of a quantity on the surface(s).

Vertex Average

turns on the computation of the vertex-averaged quantity on the surface(s).

Vertex Minimum

turns on the computation of the vertex minimum of a quantity on the surface(s).

Vertex Maximum

turns on the computation of the vertex maximum of a quantity on the surface(s).

Volume Flow Rate

turns on the computation of the volume flow rate through the surface(s).

Custom Vectors

allows you to define custom vectors if you selected Custom Vector Based Flux, Custom Vector Flux, or

Custom Vector Weighted Average from the Report Type drop-down list.

contains a list of the field variables that can be used in the surface integrations.This option is not active

if the Area, Mass Flow Rate, or Volume Flow Rate option is active.

Surfaces

is a selectable list of surfaces.

Area

displays the result of the area summation over all the selected surfaces.This label is visible when Area is

active.

displays the result of the area-weighted average computation over all the selected surfaces.This label is

visible when Area-Weighted Average is active.

Average of Facet Values

displays the result of the facet-averaged computation over all the selected surfaces.This label is visible

when Facet Average is active.

Minimum of Facet Values

displays the minimum facet value on all the selected surfaces.This label is visible when Facet Minimum

is active.

Maximum of Facet Values

is active.

displays the maximum facet value on all the selected surfaces.This label is visible when Facet Maximum

is active.

Flow Rate

displays the result of the flow rate computation over all the selected surfaces.This label is visible when

Flow Rate is active.

Integral

displays the result of the integral computation over all the selected surfaces.This label is visible when

Integral is active.

displays the result of the mass flow rate computation over all the selected surfaces.This label is visible

when Mass Flow Rate is active.

displays the result of the mass-averaged computation over all the selected surfaces.This label is visible

when Mass-Weighted Average is active.

displays the result of the standard deviation computation over all the selected surfaces.This label is visible

when Standard Deviation is active.

Sum of Facet Values

displays the result of the summation over all the selected surfaces.This label is visible when Sum is active.

Uniformity Index Mass-Wt.

displays the mass-weighted uniformity index value on all the selected surfaces.This label is visible when

Uniformity Index - Mass Weighted is active.

Uniformity Index Area-Wt.

displays the area-weighted uniformity index value on all the selected surfaces.This label is visible when

Uniformity Index - Area Weighted is active.

Average of Surface Vertex Values

displays the result of the vertex-averaged computation over all the selected surfaces.This label is visible

when Vertex Average is active.

Minimum of Vertex Values

displays the minimum facet value on all the selected surfaces.This label is visible when Vertex Minimum

is active.

Maximum of Vertex Values

displays the maximum facet value on all the selected surfaces.This label is visible when Vertex Maximum

is active.

Volumetric Flow Rate

displays the result of the volumetric flow rate computation over all the selected surfaces.This label is

visible when Volume Flow Rate is active.

Highlight Surfaces

when enabled highlights the surfaces (selected in the Surface Integrals dialog box) in the graphics

window.

Compute

computes the specified integration on the selected surfaces.

Write...

The Volume Integrals dialog box allows you to compute the volume, sum, maximum, minimum,

volume integral, volume-averaged quantity, mass integral, or mass-averaged quantity of a specified

field variable on a selected list of cell zones. See Volume Integration (p. ) for details.

Controls

contains option buttons that control the method of volume integration.

Mass-Average

turns on the computation of the mass-averaged quantity on the cell zone.

turns on the computation of the mass integral on the cell zone.

Mass

turns on the computation of the total mass in the cell zone for the selected phase.

Sum

turns on the computation of the summation over all cells in the selected zone.

Sum*2Pi

Sum

Sum*2Pi

computes the summation over all cells in the selected zone of a 2D axisymmetric model and multiplies

the result by 2π to give the summation over the revolved domain. This option is only available in 2D

axisymmetric cases.

Minimum

computes the minimum value of the selected variable at each cell in the selected zone.

Maximum

computes the maximum value of the selected variable at each cell in the selected zone.

Volume

turns on the computation of the cell zone volume.

turns on the computation of the volume integral on the cell zone.

Volume-Average

turns on the computation of the volume-weighted average on the cell zone.

contains a list of the field variables that can be used in the sum, volume integral, and average computations.

This option is not active if the Volume option is active.

Cell Zones

is a selectable list of cell zones.

Total Volume

displays the result of the volume computation over all the selected zones.This label is visible when

Volume is active.

Sum

displays the result of the summation over all the selected zones.This label is visible when Sum is active.

Sum *2Pi

displays the result of the summation over all the selected zones multiplied by 2π. This label is visible when

Sum*2Pi is active.

Max

displays the result of the maximum value of the selected zone(s).This label is visible when Maximum is

active.

Min

displays the result of the minimum value of the selected zone(s).This label is visible when Minimum is

active.

Total Volume Integral

displays the result of the volume-integral computation over all the selected zones.This label is visible

when Volume Integral is active.

active.

Volume-Weighted Average

displays the result of the volume-averaged computation over all the selected zones.This label is visible

when Volume-Average is active.

Total Mass-Weighted Integral

displays the result of the mass-integral computation over all the selected zones.This label is visible when

Mass Integral is active.

displays the result of the mass-averaged computation over all the selected zones.This label is visible

when Mass-Average is active.

Compute

computes the specified integration on the selected zones.

Write...

The Sample Trajectories dialog box allows the writing of particle states (position, velocity, diameter,

temperature, and mass flow rate) at various boundaries and planes (lines in 2D). See Sampling of Tra-

jectories (p. ) for details about the items below.

Controls

lists boundaries that can be chosen as the surfaces at which samples will be written.

Lines

(in 2D) lists lines that can be chosen as the surfaces at which samples will be written.

Planes

(in 3D) lists planes that can be chosen as the surfaces at which samples will be written.

Release From Injections

lists injections from which the injection to be tracked is chosen.

Append Files

causes the results of multiple calculations to be appended to a single file.

Accumulate Erosion/Accretion Rates

causes erosion and accretion rates to be accumulated for repeated trajectory calculations.

Sort Sample Files

causes the sample files to be sorted by injection and particle ID for steady tracking or simulated time

(flow-time in the 13th column) for unsteady tracking.The latter is required if the sample file is to be

used as an unsteady injection file.

allow control of the format and the information written for the sample output.

Output

contains a drop-down list of available user-defined functions.

Compute

causes the particles to be tracked and their status to be written to files when they encounter selected

surfaces.This button will not appear for unsteady particle tracking.

Start

initiates sampling for unsteady particle tracking.This button will replace the Compute button if you are

performing unsteady particle tracking. After you click it, it will change to the Stop button. Click Stop to

stop the sampling. (The label will change back to Start.)

The Trajectory Sample Histograms dialog box allows the plotting of histograms from sample files

created in the Sample Trajectories Dialog Box (p. ). See Histogram Reporting of Samples (p. ) for

Controls

Options

contains check buttons for histogram options.

Auto Range

toggles between automatic and manual settings of the histogram range.

Percent

causes the plot to indicate the percent of particles. Deselecting this will result in the actual number

of particles being plotted.

Histogram Mode

Percent

allows you to display the histogram with or without bars.

Weighting

allows you to apply a weight to the data sample.

Diameter Statistics

allows you to display a summary of diameter statistics for a selected variable in the console window.

allows you to choose correlations between how one particle variable depends on another particle

variable.

Cumulative Curve

allows you to compute a cumulative distribution curve for a selected variable.

(Variable^)

allows you to plot the cumulative mass distribution for a constant particle density using the particle

diameter.

Histogram Parameters

contains controls for histogram plotting.

Divisions

sets the number of “bins” in the histogram.

Min

displays the minimum value of the variable selected in the Variable list. If Auto Range is off, you can

set the minimum by typing a new value.

Max

displays the maximum value of the variable selected in the Fields list. If Auto Range is off, you can

set the maximum by typing a new value.

Axes...

opens the Axes Dialog Box (p. ), which allows you to customize the histogram axes.

Curves...

opens the Curves Dialog Box (p. ), which allows you to customize the curves used in the histogram.

Sample

lists the data samples that have been read in.

Variable

lists the fields variables available in the selected sample.

Scale, No. of Bins

is an informational list that displays the scaling and the number of bins for each variable in the selected

sample.This list is displayed only if Data File Reduction is selected.

Weight

Weight

lists the weighted fields variables available in the selected sample.

lists the sampled variables, allowing you to choose the correlation variable.

Data File Reduction

enables the reduction of injection data in the selected sample and expands the dialog box to show inputs

for Data Reduction Settings For Selected Variables and Data Reduction Options. For information

about available data reduction settings, see Data Reduction of Samples (p. ).

Plot

displays the histogram in the active graphics window.

Write...

stores the histograms in an XY-plot file format

Compute

updates the Min and Max values.

Read...

opens The Select File Dialog Box (p. ), where you can select a sample file to be read.

Reduce...

reduces sample data in the selected sample. For more information, see Data Reduction of Samples (p. ).

This button is available only if Data File Reduction is selected.

Delete

removes the sample selected in the Sample list.

The Particle Summary dialog box allows you to report a summary for particle injections. See Summary

Reporting of Current Particles (p. ) for details about the items below.

Controls

lists the particle injection(s) for which you can generate a summary.

Summary

prints the injection summary in the console window.

The Heat Exchanger Report dialog box allows you to report a summary for heat exchangers. See

Postprocessing for the Heat Exchanger Model (p. ) for details about the items below.

Controls

Options

Controls

Options

lists the available reporting options for the heat exchanger.

allows you to report the heat rejection calculated from the heat exchanger.

allows you to report the inlet temperature for both the primary and the auxiliary heat exchanger fluid.

allows you to report the outlet temperature for both the primary and the auxiliary heat exchanger

fluid.

allows you to report the mass flow rate for both the primary and the auxiliary heat exchanger fluid.

allows you to report the specific heat for both the primary and the auxiliary heat exchanger fluid.

Result

displays the results of the calculations once the Compute button is selected.

displays a list of heat exchanger fluid zones

Fluid Zone

(not available when Computed Heat Rejection option is selected.) allows you to report quantities for

either the primary or auxiliary fluid zones.

Compute

computes the specified quantity on the selected zones.

Write...

The Parameters dialog box allows you to create input parameters (in Scheme or user-defined function

procedures only) and output parameters, which allow you to compare reporting values for different

cases, or include reporting values in the function minimized by the mesh morpher/optimizer. See

Creating Output Parameters (p. ) for details about the items below.

Controls

Input Parameters

Controls

contains a list of existing input parameters. See Defining and Viewing Parameters (p. ) for details about

creating input parameters.

Edit...

opens the Parameter Expression Dialog Box (p. ).

Important

When using ANSYS Fluent  in ANSYS Workbench, parameters are not editable, so the

Edit... button becomes the View... button. This opens the Parameter Expression Dialog

Box (p. ) where the parameter properties can only be viewed. For more information,

see the separate ANSYS Fluent in Workbench User’s Guide.

Delete

removes the selected input parameter from the list of Input Parameters.

More

contains a drop-down list that allows more advanced use of input parameters. Available options

include:

opens the Use Input Parameter in Scheme Procedure Dialog Box (p. ).

Use in UDF

opens the Use Input Parameter for UDF Dialog Box (p. ).

Output Parameters

contains a list of existing output parameters.

Create

opens the Report Definitions Dialog Box (p. ), allowing you to create additional output parameters

based on report definitions.

Edit...

opens the dialog box corresponding to the selected item in the Output Parameters list.

More

contains a drop-down list containing additional tasks that you can perform, including:

Delete

Rename

reports values to the console window. If you select multiple output parameters, then the output in-

cludes values from multiple output parameters.

Write...

Note

ANSYS Fluent automatically creates generic default names for new input and output para-

meters (for example, parameter-, parameter-, parameter-, and so on) If a

parameter is deleted, the default name is not reused. For example, if you have parameter-

, parameter-, and parameter-, then delete parameter- and create a new

parameter, the default name for the new parameter will be parameter-.

The Use Input Parameter in Scheme Procedure dialog box allows you to use the input parameter

in a Scheme procedure. In turn, this Scheme procedure can also use text user interface (TUI) commands.

For more information, see Working With Advanced Parameter Options (p. ).

Controls

Input Parameter

contains the name of an input parameter.

Select

opens the Select Input Parameter Dialog Box (p. ) where an input parameter can be chosen.

Scheme Procedure (Single Real Argument)

contains a procedure name (if already defined using a Scheme file) or procedure body written in the

Scheme language using lambda.This procedure should receive one real argument.

Define

registers the selected input parameter.

Registered List

contains a list of registered input parameters.

Delete

Define

Delete

removes a selected registered input parameter from the list.

Print

prints details of the registered input parameters.

The Use Input Parameter for UDF dialog box allows you to select the input parameters that can be

used inside a user-defined function (UDF) during calculations.

Controls

Select

Define

Delete

Print

prints the ID of the registered input parameters.The ID values are used to access the value of the para-

meter in the user-defined function.

The Rename dialog box allows you to change the name of the output parameter that you created.

Controls

New Name

contains the new name of the output parameter.

The Parameter Expression dialog box allows you to create input parameters, which can be used to

run a case and vary the value of the input to explore how the results change.

Controls

Name

contains the name of the input parameter expression.

contains the current value of the input parameter.

Used In

indicates the cell zone or boundary condition where the input parameter is currently used.The relevant

zone or boundary condition will be displayed after you create an input parameter.

Important

Important

Note

meters (for example, parameter_1, parameter_2, parameter_3, and so on) If a

parameter is deleted, the default name is not reused. For example, if you have paramet-

The Save Output Parameter dialog box allows you to save specific output parameters that allow you

to compare reporting values for different cases. See Creating Output Parameters (p. ) for details

Controls

Options

contains options for saving your output parameters.

Create New Output Parameter

allows you to create a new output parameter.

Apply Report Settings to an Existing Output Parameter

allows you to overwrite an existing output parameter of the same type.

Name

contains the name for the current output parameter.

Note

The Parameters and Customization task page introduces you to the parameterization and customization

tools available for use in solving your CFD simulation using ANSYS Fluent.

Chapter : Ribbon Reference Guide

This reference guide provides information about the ribbon in ANSYS Fluent.

.. File Ribbon Tab

.. Dialog Boxes Available from the Ribbon

... File/Read/Mesh...

... File/Read/Case...

... File/Read/Data...

... File/Read/Case & Data...

... File/Read/PDF...

... File/Read/ISAT Table...

... File/Read/DTRM Rays...

... File/Read/View Factors...

... File/Read/Profile...

... File/Read/Scheme...

... File/Read/Journal...

... File/Write/Case...

... File/Write/Data...

... File/Write/Case & Data...

... File/Write/PDF...

... File/Write/ISAT Table...

... File/Write/Flamelet...

... File/Write/Surface Clusters...

... File/Write/Profile...

... File/Write/Autosave...

... File/Write/Boundary Mesh...

... File/Write/Start Journal...

... File/Write/Stop Journal

... File/Write/Start Transcript...

... File/Write/Stop Transcript

... File/Import/ABAQUS/Input File...

... File/Import/ABAQUS/Filbin File...

... File/Import/ABAQUS/ODB File...

... File/Import/CFX/Definition File...

... File/Import/CFX/Result File...

... File/Import/CGNS/Mesh...

... File/Import/CGNS/Data...

... File/Import/CGNS/Mesh & Data...

... File/Import/EnSight...

... File/Import/FIDAP...

... File/Import/GAMBIT...

... File/Import/HYPERMESH ASCII...

... File/Import/I-deas Universal...

... File/Import/LSTC/Input File...

... File/Import/LSTC/State File...

... File/Import/Marc POST...

... File/Import/Mechanical APDL/Input File...

... File/Import/Mechanical APDL/Result File...

... File/Import/NASTRAN/Bulkdata File...

... File/Import/NASTRAN/Op2 File...

... File/Import/PATRAN/Neutral File...

... File/Import/PLOT3D/Grid File...

... File/Import/PLOT3D/Result File...

... File/Import/PTC Mechanica Design...

... File/Import/Tecplot...

... File/Import/Fluent  Case File...

... File/Import/PreBFC File...

... File/Import/Partition/Metis...

... File/Import/Partition/Metis Zone...

... File/Import/CHEMKIN Mechanism...

... File/Export/Solution Data...

... File/Export/Particle History Data...

... File/Export/During Calculation/Solution Data...

... File/Export/During Calculation/Particle History Data...

... File/Export to CFD-Post...

... File/Solution Files...

... File/Interpolate...

... File/FSI Mapping/Volume...

... File/FSI Mapping/Surface...

... File/Save Picture...

... File/Data File Quantities...

... File/Batch Options...

... File/Exit

The File/Read/Mesh... ribbon tab item opens the Read Mesh Options Dialog Box (p. ), which allows

you to read or replace a mesh.

.... Read Mesh Options Dialog Box

The Read Mesh Options dialog box is used to read or replace a mesh. See Reading Mesh Files (p. )

Ribbon Reference Guide

Controls

Options

allows you to read in a new mesh or replace the existing mesh.

Discard Case And Data, Read New Mesh

Controls

Options

results in both the case and data files being discarded when reading in a new mesh.

Discard Data, Replace Mesh

results in the data file being discarded when replacing an existing mesh.

Show Scale Mesh Panel After Replacing Mesh

gives you the option to have the Scale Mesh Dialog Box (p. ) appear automatically for you to check

or scale your mesh.

The File/Read/Case... ribbon tab item is used to read in an ANSYS Fluent case file (extension .cas),

or a mesh file (extension .msh, .grd, .MSH, or .GRD) that has been saved in the native format for

ANSYS Fluent. See Reading Mesh Files (p. ) and Reading and Writing Case and Data Files (p. ) for

details.

The File/Read/Case... ribbon tab item opens The Select File Dialog Box (p. ), which allows you to

select the appropriate file to be read.

File Ribbon Tab

The File/Read/Data... ribbon tab item is used to read in an ANSYS Fluent data file (which has a .dat

extension). This item will not be available until you read in a case or mesh file. See Reading and Writing

Data Files (p. ) for details.

The File/Read/Data... ribbon tab item opens The Select File Dialog Box (p. ), which allows you to

The File/Read/Case & Data... ribbon tab item is used to read in an ANSYS Fluent case file and the

corresponding data file (for example, myfile.cas and myfile.dat) together. See Reading and

Writing Case and Data Files Together (p. ) for details.

The File/Read/Case & Data... ribbon tab item opens The Select File Dialog Box (p. ), which allows

you to select the appropriate files to be read. Select the appropriate case file, and the corresponding

data file (that is, the file having the same name with a .dat extension) will also be read in.

The File/Read/PDF... ribbon tab item is used to read a PDF file (extension .pdf) created by ANSYS

Fluent for use with the non-premixed or partially premixed combustion model. This item is available

only when the non-premixed or partially premixed combustion model has been enabled. See Saving

the Look-Up Tables (p. ) for details.

The File/Read/ISAT Table... ribbon tab item is used to read an ISAT table (extension .isat) for use

with the Composition PDF Transport model. This item is available only when the Composition PDF

Transport model has been enabled. See Using ISAT Efficiently (p. ) for details.

The File/Read/DTRM Rays... ribbon tab item is used to read a ray file (extension .ray) created by

ANSYS Fluent for use with the DTRM (radiation model). This item is available only when the DTRM has

been enabled. See Writing and Reading the DTRM Ray File (p. ) for details.

The File/Read/View Factors... ribbon tab item is used to read in a view factor file for use with the

surface-to-surface (S2S) radiation model. This item is available only when the S2S model has been en-

abled. See Reading View Factors into ANSYS Fluent (p. ) for details.

The File/Read/Profile... ribbon tab item opens the Select File dialog box for reading profiles (Reading

Profile Files (p. )), It is used to read a cell zone or boundary condition profile file (extension .prof).

A profile file defines profiles that can be used to specify flow conditions for a cell zone or a boundary.

See Profiles (p. ) for details.

The File/Read/Scheme... ribbon tab item is used to read in a Scheme source file (extension .scm).

See Reading Scheme Source Files (p. ) for details.

The File/Read/Journal... ribbon tab item is used to read in a journal file (extension .jou) containing

a sequence of ANSYS Fluent commands. You can create a journal file using the File/Write/Journal...

ribbon tab item. See Creating and Reading Journal Files (p. ) for details.

The File/Write/Case... ribbon tab item is used to save an ANSYS Fluent case file. See Reading and

Writing Case Files (p. ) for details.

The File/Write/Case... ribbon tab item opens The Select File Dialog Box (p. ), which allows you to

save the file with a name of choice. The dialog box is similar to the Select File dialog box for reading

files, except that it has an additional option for writing binary files.

Important

When ANSYS Fluent writes a case file, the .cas extension is added to the file name specified,

You can also write a compressed file by appending .gz or .Z to the file name. (See Reading

and Writing Compressed Files (p. ) for details about file compression.)

The File/Write/Data... ribbon tab item is used to save an ANSYS Fluent data file (which has a .dat

extension). See Reading and Writing Data Files (p. ) for details.

Important

When ANSYS Fluent writes a data file, the .dat extension is added to the file name specified,

unless the name already ends with .dat.

You can compress data files by appending .gz or .Z to the file name (see Reading and Writing

Compressed Files (p. ) for details about file compression).

The File/Write/Case & Data... ribbon tab item is used to save an ANSYS Fluent case file and data file

at the same time (for example, myfile.cas and myfile.dat). See Reading and Writing Case and

Data Files Together (p. ) for details.

Enter the name of the case file in the text entry box in the Select File dialog box and the corresponding

data file (same file name, but with a .dat extension) will also be written.

The File/Write/PDF... ribbon tab item is used to write a PDF file after computing the look-up tables

using the non-premixed or partially premixed combustion model in ANSYS Fluent. This item is available

The File/Write/ISAT Table... ribbon tab item is used to write an ISAT table. See Using ISAT Effi-

ciently (p. ) for details.

The File/Write/Flamelet... ribbon tab item is used to write a flamelet file generated using the non-

premixed or partially premixed combustion model in ANSYS Fluent. This item is available only when

the non-premixed or partially premixed combustion model has been enabled. See The Diffusion

Flamelet Models Theory in the Theory Guide for details.

The File/Write/Surface Clusters... ribbon tab item is used to set parameters related to surface clusters

and view factors for the surface-to-surface radiation model. It opens the View Factors and Clustering

Dialog Box (p. ). The dialog box that you open using the File/Write/Surface Clusters... ribbon tab

item is different than the one opened via the Settings... button in the Radiation Model dialog box,

in that it saves the settings you specify to a file that can be used to calculate the view factors outside

of ANSYS Fluent (see Computing View Factors Outside ANSYS Fluent (p. )). When you click OK, The

Select File Dialog Box (p. ) will open so that you can specify a name for the file where ANSYS Flu-

ent should save the settings.

The File/Write/Profile... ribbon tab item opens the Write Profile Dialog Box (p. ).

The File/Write/Autosave... ribbon tab item opens the Autosave Dialog Box (p. ).

The File/Write/Boundary Mesh... ribbon tab item is used to write the boundary zones (surface mesh)

of the domain to a file. You can then read this file into the meshing mode of Fluent or GAMBIT to

produce an improved volume mesh. See Writing a Boundary Mesh (p. ) for details.

The File/Write/Start Journal... ribbon tab item is used to start the recording of subsequent ANSYS

Fluent commands to a journal file. You can read this journal file back into Fluent later (using the

File/Read/Journal... ribbon tab item) to automate the execution of the recorded commands. See

Creating and Reading Journal Files (p. ) for details.

The File/Write/Stop Journal ribbon tab item replaces the File/Write/Start Journal... ribbon tab item

after the recording of a journal file has begun. The File/Write/Stop Journal ribbon tab item is used

to end the journal recording. See Creating and Reading Journal Files (p. ) for details.

The File/Write/Start Transcript... ribbon tab item is used to start the recording of a transcript file

containing all input to and output from Fluent. (You cannot read a transcript file back into Fluent.)

See Creating Transcript Files (p. ) for details.

The File/Write/Stop Transcript ribbon tab item replaces the File/Write/Start Transcript... ribbon tab

item after the recording of a transcript file has begun. The File/Write/Stop Transcript ribbon tab item

is used to end the transcript recording. See Creating Transcript Files (p. ) for details.

The File/Import/ABAQUS/Input File... ribbon tab item is used to import an ABAQUS input file (extension

.inp), which contains the input description of a finite element model for the ABAQUS finite element

program. See ABAQUS Files (p. ) for details.

The File/Import/ABAQUS/Filbin File... ribbon tab item is used to import an ABAQUS filbin file (extension

.fil), which contains the finite element model and results data. See ABAQUS Files (p. ) for details.

The File/Import/ABAQUS/ODB File... ribbon tab item is used to import an ABAQUS ODB file with a

.odb extension. See ABAQUS Files (p. ) for details.

The File/Import/CFX/Definition File... ribbon tab item is used to import a CFX definition file (extension

.def), which contains mesh information to be read into Fluent. See CFX Files (p. ) for details.

The File/Import/CFX/Result File... ribbon tab item is used to import a CFX result file (extension .res).

See CFX Files (p. ) for details.

The File/Import/CGNS/Mesh... ribbon tab item is used to read in a CGNS-format mesh file (extension

.cgns). See Meshes and Data in CGNS Format (p. ) for details.

The File/Import/CGNS/Data... ribbon tab item is used to read in a CGNS-format data file. See Meshes

and Data in CGNS Format (p. ) for details.

The File/Import/CGNS/Mesh & Data... ribbon tab item is used to read in a set of CGNS-format mesh

and data files. See Meshes and Data in CGNS Format (p. ) for details.

The File/Import/EnSight... ribbon tab item is used to import EnSight files (extension .encas or

.case). See EnSight Files (p. ) for details.

The File/Import/FIDAP... ribbon tab item is used to import an ANSYS FIDAP neutral file (extension

.FDNEUT or .unv). See ANSYS FIDAP Neutral Files (p. ) for details.

The File/Import/GAMBIT... ribbon tab item is used to read in a neutral file from GAMBIT. See GAMBIT

and GeoMesh Mesh Files (p. ) for details.

The File/Import/HYPERMESH ASCII... ribbon tab item is used to import a HYPERMESH ASCII file

(extension .hm, .hma, or .hmascii). See HYPERMESH ASCII Files (p. ) for details.

The File/Import/I-deas Universal... ribbon tab item is used to import an I-deas Universal file, which

contains mesh information and zone types to be read into Fluent. See I-deas Universal Files (p. ) for

details.

The File/Import/LSTC/Input File... ribbon tab item is used to import an LSTC input file (extension .k,

.key, or .dyn), which contains the input description of a finite element model for the LS-DYNA finite

element program. See LSTC Files (p. ) for details.

The File/Import/LSTC/State File... ribbon tab item is used to import an LSTC state file (extension

.d3plot), which contains control data, geometry data, and state data. See LSTC Files (p. ) for details.

The File/Import/Marc POST... ribbon tab item is used to import a Marc POST file generated using the

MSC Marc finite element program. See Marc POST Files (p. ) for details

The File/Import/Mechanical APDL/Input File... ribbon tab item is used to import a Mechanical AP-

DL input file (extensions .ans, neu, .cdb, or .prep7), which contains mesh information to be read

into Fluent. See Mechanical APDL Files (p. ) for details.

The File/Import/Mechanical APDL/Result File... ribbon tab item is used to import a Mechanical AP-

DL result file (extension .rst, .rth, or .rmg). See Mechanical APDL Files (p. ) for details.

The File/Import/NASTRAN/Bulkdata File... ribbon tab item is used to import a NASTRAN Bulkdata

file (extension .nas, .dat, or .bdf), which contains mesh information to be read into Fluent. See

NASTRAN Files (p. ) for details.

The File/Import/NASTRAN/Op2 File... ribbon tab item is used to import a NASTRAN Op2 file (extension

.op2), which is an output binary data file containing data used in the NASTRAN finite element program.

See NASTRAN Files (p. ) for details.

The File/Import/PATRAN/Neutral File... ribbon tab item is used to read in a PATRAN Neutral file (ex-

tension .neu, .out, or .pat) zoned by named components (that is, with the nodes placed into zones

based on group name). The PATRAN neutral file contains mesh information to be read into Fluent. See

PATRAN Neutral Files (p. ) for details.

The File/Import/PLOT3D/Grid File... ribbon tab item is used to import a PLOT3D grid file (extension

.g, .x, .xyz, or .grd). See PLOT3D Files (p. ) for details.

The File/Import/PLOT3D/Result File... ribbon tab item s used to import a PLOT3D result file (extension

The File/Import/PTC Mechanica Design... ribbon tab item is used to import a PTC Mechanica Design

file (extension .neu), which contains analysis, model, and results data (only in binary form). See PTC

Mechanica Design Files (p. ) for details.

The File/Import/Tecplot... ribbon tab item is used to read in a Tecplot binary file. See

Tecplot Files (p. ) for details.

The File/Import/Fluent  Case File... ribbon tab item is used to read in a case file created in FLUENT

. See Fluent  Case Files (p. ) for details.

The File/Import/PreBFC File... ribbon tab item is used to read in a structured (quadrilateral or hexa-

hedral) mesh that was created using PreBFC. See PreBFC Files (p. ) for details.

The File/Import/Partition/Metis... ribbon tab item is used to partition a mesh and then read it into

the parallel version of ANSYS Fluent. See Using the Partition Filter (p. ) for an explanation of the

difference between this item and the File/Import/Partition/Metis Zone... ribbon tab item.

The File/Import/Partition/Metis Zone... ribbon tab item is used to partition each cell zone in a mesh

individually and then read the mesh into the parallel version of ANSYS Fluent. See Using the Partition

Filter (p. ) for an explanation of the difference between this item and the File/Import/Partition/Met-

is... ribbon tab item.

The File/Import/CHEMKIN Mechanism... ribbon tab item opens the Import CHEMKIN Format Mech-

anism Dialog Box (p. ).

.... Import CHEMKIN Format Mechanism Dialog Box

The Import CHEMKIN Format Mechanism dialog box is used to import a CHEMKIN-format chemical

mechanism file into ANSYS Fluent. See Importing a Volumetric Kinetic Mechanism in CHEMKIN

Format (p. ) for details. The dialog box can be accessed either from the Species Model Dialog

Box (p. ) or from the main menu:

Controls

specifies a name for the material.

Gas-Phase

contains inputs for importing the gas-phase mechanism in CHEMKIN format.

Kinetics Input File

specifies the name of the gas-phase file in CHEMKIN-format. If the file is not in the current working

folder, include the full path to the folder where it is located.

Thermodynamic Database

specifies thermodynamic property data for species whose thermodynamic data are not specified in

the kinetics input file.You can enable All contained in Kinetics Input Files to indicate that the

kinetics input file contains the thermodynamic data for all the species.

Transport Property Data (Optional)

(if Import database is enabled) allows you to specify transport property data for species whose

transport data are not specified in the kinetics input file.You can enable All contained in Kinetics

Input Files to indicate that the kinetics input file contains the transport data for all the species.

Import Surface Mechanism

enables the importing of the surface mechanism.

Surface

contains inputs for importing the surface mechanism.This group box appears only when the Import

Surface Mechanism option is enabled.

specifies the name of the surface kinetics CHEMKIN-format file.

specifies whether the thermodynamic data for the surface-chemistry species will be included in the

surface kinetics CHEMKIN-format file (if All contained in Kinetics Input File is enabled or in the

thermodynamic database file specified in the Gas-Phase group box (if Same as 'Gas-Phase' is en-

abled). Note that if no thermodynamic database file is specified in the Gas-Phase group box, the

thermodynamic data for all surface-chemistry species must be included the surface kinetics input

file.

Import

imports the specified Chemkin reaction mechanism and thermal files and saves the imported data in

the Fluent case file. Note that carrying the original input files along with the Fluent case file is not required.

ANSYS Fluent will automatically regenerate these files when needed (for example, when using the

CHEMKIN-CFD solver).

The File/Export/Solution Data... ribbon tab item opens the Export Dialog Box (p. ).

.... Export Dialog Box

The Export dialog box allows you to write data that can be read by other data visualization and

postprocessing tools. See Exporting Solution Data (p. ) for a complete description of the available

data formats and how to use the dialog box.

Controls

File Type

contains a drop-down list that controls the output file format that will be written using the Write...

button.

ABAQUS

ASCII

allows you to specify the surface(s), scalars, location in the cell from which the values of scalar functions

are to be taken, and the delimiter separating the fields, to be exported to an ASCII file.

AVS

allows you to specify the cell zones, surfaces, quantities, format (Binary or ASCII), and whether a

case file is written for data export.The .cdat file format is compatible with both CFD-Post and En-

Sight.

CGNS

FAST

allows you to specify the scalars you want to write and the cell zones or surfaces from which the

values of scalar functions are to be taken, to be exported to a FIELDVIEW binary file (extension

.fvuns) and a regions file (extension .fvuns.fvreg).

Note

You must deselect all cell zones before you can select any surfaces.

NASTRAN

PATRAN

PATRAN

TAITherm

Tecplot

Cell Zones

specifies the cell zones for which data is to be written for a CFD-Post compatible, EnSight, or FIELDVIEW

file.

Surfaces

specifies valid functions for output.The attributes of the list are modified based on the active file type.

The list may be a single-selection or a multiple-selection list or it may be disabled, depending on the

selected File Type.

contains optional structural loads that can be written to ABAQUS, I-deas Universal, Mechanical APDL

Input, NASTRAN, and PATRAN files.This option is available only when Structural analysis is selected.

Force

Pressure

enables temperature to be written as a load for a structural analysis.This option is available only

when the Energy Equation is enabled.

Heat Flux

specifies the location in the cell from which the values of scalar functions are to be taken.

Node

Analysis (for ABAQUS, I-deas Universal, Mechanical APDL Input, NASTRAN, and PATRAN formats

Thermal

Delimiter (for ASCII format only)

specifies the delimiter used to separate the data fields.

Comma

specifies comma as the delimiter separating the data fields.

Space

specifies space as the delimiter separating the data fields.

Transient (for EnSight Case Gold only)

contains options for exporting transient data.

Transient

enables export of transient data.

Transient

Separate Files for Each Timestep

enables writing separate files for each timestep.

Append Frequency

specifies the frequency for appending the data during the solution process.

Important

The Append Frequency option is replaced by the Write Frequency option when

Separate Files for Each Timestep is enabled. You can specify the frequency for

writing the separate files.

File Name

Format (for EnSight Case Gold and CDAT for CFD-Post & EnSight)

Binary

ASCII

Flux Based

Write Case File (for CDAT for CFD-Post & EnSight only)

specifies whether or not a case file is written with the .cdat file.

Write...

opens The Select File Dialog Box (p. ) for writing the specified function(s) in the specified format.

The File/Export/Particle History Data... ribbon tab item opens the Export Particle History Data Dialog

Box (p. ).

.... Export Particle History Data Dialog Box

The Export Particle History Data dialog box allows you to export particle history data as your solution

progresses. See Exporting Steady-State Particle History Data (p. ) for details.

Controls

Type

CFD-Post

FieldView

EnSight

Geometry

allows you to write the file in .ibl format, which can be read in GAMBIT (not available when Un-

steady Particle Tracking is enabled in the Discrete Phase dialog box, which is opened by clicking

Discrete Phase... in the Physics ribbon tab).

Quantity

Skip

Coarsen

reduces the exported file size by reducing the number of points that are written for a given trajectory.

This is only valid for steady-state cases.

Encas File Name

is the file name you will specify if you selected EnSight under Type. Use the Browse... button to select

the .encas file that was created when you exported the file with the File/Export... ribbon tab option.

Number of Particle Time Steps

appears when you select EnSight under Type.The specified number is the number of particle time-

steps that are saved to the .encas file.

The File/Export/During Calculation/Solution Data... ribbon tab item opens the Automatic Export

Dialog Box (p. ) (transient cases only).

The File/Export/During Calculation/Particle History Data... ribbon tab item opens the Automatic

Particle History Data Export Dialog Box (p. ) (transient cases only).

The File/Export to CFD-Post... ribbon tab item opens the Export to CFD-Post Dialog Box (p. ).

.... Export to CFD-Post Dialog Box

The Export to CFD-Post dialog box allows you to select the quantities that you would like to export

to CFD-Post. See Exporting to ANSYS CFD-Post (p. ) for details.

Controls

Select Quantities

contains a selectable list where you can choose the quantities to export.

Format

allows you to export the .cdat file in Binary or ASCII format.

Write Case File

Open CFD-Post

specifies that after the files have been written, a CFD-Post session is opened, with the case and .cdat

files loaded. CFD-Post will display the results.

Write...

opens the Select File dialog box, where you can specify the name and location of the exported files.

The File/Solution Files... ribbon tab item opens the Solution Files Dialog Box (p. ).

.... Solution Files Dialog Box

The Solution Files dialog box allows you to manage the files that were created through the Autosave

Dialog Box (p. ). See Managing Solution Files (p. ) for details.

Controls

Solution Files at

contains a selectable list where you can choose the files to read or delete.

Read

makes the selected file the current file. Note that if more than one file is selected, the Read button is

disabled.When an earlier solution is made current, the solution files that were generated for a later iter-

ation/time-step will be removed from this list when the calculation continues.

Delete

removes the selected solution files.

File Names...

allows you to obtain information about the solution files and the path of the associated files.

Recover Missing Solution...

Recovers the latest case and data files from the system folder (<project name>\dp0\FFF\Fluent\

for analysis system and <project name>\dp0\ FLU \Fluent\ for component system) and list

them in the Solution Files at list. (This option is available only in Fluent used under Workbench.)

The File/Interpolate... ribbon tab item opens the Interpolate Data Dialog Box (p. ).

.... Interpolate Data Dialog Box

The Interpolate Data dialog box allows you to interpolate solution data from one mesh to another.

See Mesh-to-Mesh Solution Interpolation (p. ) for details.

Controls

Options

contains the interpolation options.

Read and Interpolate

allows you to read and interpolate solution data onto the current mesh.

Write Data

allows you to write an interpolation file for the solution data to be interpolated onto another mesh.

Cell Zones

is a list of cell zones that can be selected.

Write Data

Cell Zones

Binary File

allows you to write binary interpolation files.This option is available only when Write Data is selected

Fields

is a list of all available data fields that can be selected.This list is available only when Write Data is se-

lected under Options.

Read...

opens The Select File Dialog Box (p. ), in which you can specify the file to be read.This button is

available only when the Read and Interpolate option is selected.

Write...

opens The Select File Dialog Box (p. ), in which you can specify a name for the file to be saved and

then save the file.This button replaces the Read... button when the Write Data option is selected.

The File/FSI Mapping/Volume... ribbon tab item opens the Volume FSI Mapping Dialog Box (p. ).

....Volume FSI Mapping Dialog Box

The Volume FSI Mapping dialog box allows you to map cell data for a given geometry from an ANSYS

Fluent file onto a file with a different mesh and format. See Mapping Data for Fluid-Structure Interaction

(FSI) Applications (p. ) for a complete description of how to use the dialog box.

Controls

Input File

contains parameters related to the input file.

Type

contains the options for the format of the input mesh file.

ABAQUS

specifies that an ABAQUS file will be used as the input mesh file (extension .inp).

I-deas

specifies that an I-deas file will be used as the input mesh file (extension .unv).

specifies that a Mechanical APDL file will be used as the input mesh file (extension .cdb or

.neu).

.neu).

NASTRAN

specifies that a NASTRAN file will be used as the input mesh file (extension .bdf).

PATRAN

specifies that a PATRAN file will be used as the input mesh file (extension .neu, .out, or .pat).

FEA File

specifies the name of the input mesh file (see the Input File Type descriptions for associated file

extensions). If the file is not in the current working folder, include the full path to the folder where

it is located.

Browse...

opens The Select File Dialog Box (p. ), which you can use to specify the input mesh file instead of

entering it in the Input File text-entry box.

Length Units

specifies the unit of length used in the input file.

Display Options

allows you to choose either the FEA Mesh or the ANSYS Fluent Mesh (or both).

Analysis

contains the options for the kind of data to be mapped.

specifies that data fields relevant for a structural analysis will be mapped.

Thermal

specifies that data fields relevant for a thermal analysis will be mapped.

consists of a list of available loads, including Force, Pressure, and Temperature.

Fluent Zones

contains a list of available cell zones from the current ANSYS Fluent file from which cell data will be

mapped.

contains the options for the format of the file that will be created from the input mesh file and the

mapped data.

Type

contains the options for the format of the output mesh file.

ABAQUS

specifies that an ABAQUS file will be used as the output mesh file (extension .inp).

I-deas

specifies that an I-deas file will be used as the output mesh file (extension .unv).

I-deas

specifies that a Mechanical APDL file will be used as the output mesh file (extension .cdb).

NASTRAN

specifies that a NASTRAN file will be used as the output mesh file (extension .bdf).

PATRAN

specifies that a PATRAN file will be used as the output mesh file (extension .out).

File Name

specifies the name of the input mesh file (see the Output File descriptions for associated file exten-

sions). If the file is not in the current working folder, include the full path to the folder where it is

located.

Browse...

Include FEA Mesh

includes additional FEA information like node/element information in the exported output file.

specifies the unit of temperature when mapping temperature for a structural analysis or any variable

for a thermal analysis.

Read

reads the input file into memory.

Display

displays the selected mesh in the graphics window.

Write

writes an output file in which the selected ANSYS Fluent cell data is mapped onto the input mesh file.

The File/FSI Mapping/Surface... ribbon tab item opens the Surface FSI Mapping Dialog Box (p. ).

.... Surface FSI Mapping Dialog Box

The Surface FSI Mapping dialog box allows you to map face data for a given geometry from an

ANSYS Fluent file to a file with a different mesh and format. See Mapping Data for Fluid-Structure

Interaction (FSI) Applications (p. ) for a complete description of how to use the dialog box.

Controls

Input File

Type

ABAQUS

I-deas

.neu).

NASTRAN

PATRAN

FEA File

Browse...

Analysis

Thermal

Analysis

Thermal

contains a list of available face zones from the current ANSYS Fluent file from which cell data will be

mapped.

Type

ABAQUS

I-deas

NASTRAN

PATRAN

File Name

located.

Browse...

HTC Type

specifies the means of calculating the heat transfer coefficient.

ref-temp

uses a temperature equal to the reference temperature to calculate the heat transfer coefficient.

cell-temp

uses a temperature equal to the temperature of the cell adjacent to the face to calculate the

heat transfer coefficient.

Read

Display

Write

writes an output file in which the ANSYS Fluent data has been mapped to the mesh of the input file.

The File/Save Picture... ribbon tab item opens the Save Picture Dialog Box (p. ).

The File/Data File Quantities... ribbon tab item opens the Data File Quantities Dialog Box (p. ).

The File/Batch Options... ribbon tab item opens the Batch Options Dialog Box (p. ).

.... Batch Options Dialog Box

The Batch Options dialog box allows you to select options to suppress interactive dialog boxes from

ANSYS Fluent while running a case in batch mode. See Batch Execution Options (p. ) in the Getting

Started Guide for details.

Controls

Controls

determines whether ANSYS Fluent confirms a file overwrite.This option is enabled by default.

allows you to hide Question dialog boxes.This option is disabled by default.

The File/Exit ribbon tab item is used to exit from the current solver session.

The dialog boxes described in this section can be accessed through the ribbon, from the tabs other

than the File ribbon tab.

... 1D Simulation Library Dialog Box

... Activate Cell Zones Dialog Box

... Adaption Controls Dialog Box

... Adaption Display Options Dialog Box

Dialog Boxes Available from the Ribbon

... Adjacency Dialog Box

... Animation Definition Dialog Box

... Anisotropic Adaption Dialog Box

... Auto Create Options Dialog Box

... Auto Partition Mesh Dialog Box

... Boundary Adaption Dialog Box

... Cell Register Display Options Dialog Box

... Compiled UDFs Dialog Box

... Contours Dialog Box

... Convergence Conditions Dialog Box

... Create/Edit Mesh Interfaces Dialog Box

... Custom Field Function Calculator Dialog Box

... Custom Laws Dialog Box

... Deactivate Cell Zones Dialog Box

... Define Control Points Dialog Box

... Delete Cell Zones Dialog Box

... Display Options - Adaption Dialog Box

... DPM Report Definition Dialog Box

... DPM Source Report Definition

... Drag Report Definition Dialog Box

... DTRM Graphics Dialog Box

... DTRM Rays Dialog Box

... Edit Mesh Interfaces Dialog Box

... Edit Report File Dialog Box

... Edit Report Plot Dialog Box

... Execute on Demand Dialog Box

... Expression Dialog Box

... Expression Report Definition Dialog Box

... Field Function Definitions Dialog Box

... Flux Report Definition Dialog Box

... Force Report Definition Dialog Box

... Fuse Face Zones Dialog Box

... Geometry Based Adaption Controls Dialog Box

... Geometry Based Adaption Dialog Box

... Gradient Adaption Dialog Box

... Import Particle Data Dialog Box

... Imprint Surface Dialog Box

... Improve Mesh Dialog Box

... Injections Dialog Box

... Input Summary Dialog Box

... Interface Options Dialog Box

... Interpreted UDFs Dialog Box

... Iso-Clip Dialog Box

... Iso-Surface Dialog Box

... Iso-Value Adaption Dialog Box

... Lift Report Definition Dialog Box

... Line/Rake Surface Dialog Box

... Manage Adaption Registers Dialog Box

... Merge Zones Dialog Box

... Mesh Adaption Controls Dialog Box

... Mesh Interfaces Dialog Box

... Mesh Morpher/Optimizer Dialog Box

... Mixing Planes Dialog Box

... Moment Report Definition Dialog Box

... Motion Settings Dialog Box

... Multi Edit Dialog Box

... New Report File Dialog Box

... New Report Plot Dialog Box

... Objective Function Definition Dialog Box

... Optimization History Monitor Dialog Box

... Parallel Connectivity Dialog Box

... Parameter Bounds Dialog Box

... Particle Tracks Dialog Box

... Partition Surface Dialog Box

... Partitioning and Load Balancing Dialog Box

... Pathlines Dialog Box

... Plane Surface Dialog Box

... Point Surface Dialog Box

... Quadric Surface Dialog Box

... Reduced Order Model Dialog Box

... Reference Frame Dialog Box

... Region Adaption Dialog Box

... Replace Cell Zone Dialog Box

... Report Definitions Dialog Box

... Report File Definitions Dialog Box

... Report Plot Definitions Dialog Box

... Residual Monitors Dialog Box

... Rotate Mesh Dialog Box

... S2S Information Dialog Box

... Separate Cell Zones Dialog Box

... Separate Face Zones Dialog Box

... Set Injection Properties Dialog Box

... Set Multiple Injection Properties Dialog Box

... Shell Conduction Layers Dialog Box

... Shell Conduction Manager Dialog Box

... Structural Point Surface Dialog Box

... Surface Meshes Dialog Box

... Surface Report Definition Dialog Box

... Surfaces Dialog Box

...Thread Control Dialog Box

...Transform Surface Dialog Box

...Translate Mesh Dialog Box

...Turbo 2D Contours Dialog Box

...Turbo Averaged Contours Dialog Box

...Turbo Averaged XY Plot Dialog Box

...Turbo Options Dialog Box

...Turbo Report Dialog Box

...Turbo Topology Dialog Box

... UDF Library Manager Dialog Box

... User-Defined Fan Model Dialog Box

... User-Defined Function Hooks Dialog Box

... User-Defined Memory Dialog Box

... User Defined Report Definition Dialog Box

... User-Defined Scalars Dialog Box

...Vectors Dialog Box

...Volume Adaption Dialog Box

...Volume Report Definition Dialog Box

...Warning Dialog Box

...Yplus/Ystar Adaption Dialog Box

... Zone Surface Dialog Box

The 1D Simulation Library dialog box allows you to set parameters related to coupling between

ANSYS Fluent and GT-POWER or WAVE. See Coupling Boundary Conditions with GT-POWER (p. ) or

Coupling Boundary Conditions with WAVE (p. ) for details about the items below.

Controls

1D Library

specifies the type of library to be used. (Currently only GTpower and WAVE are available.)

1D Input File Name

specifies the name of the GT-POWER or WAVE input file.

Start

starts up GT-POWER or WAVE and generates ANSYS Fluent user-defined functions for each boundary in

Stop

unlinks the shared library.

The Activate Cell Zones dialog box allows you to activate a single cell zone or multiple zones. See

Activating Zones (p. ) for details.

Controls

Cell Zones

contains a list of cell zones from which you can select the zone to be activated.

Activate

activates the selected cell zones.

Controls

Cell Zones

Activate

The Adaption Controls dialog box allows you to specify the refinement and coarsening criteria that

Fluent will use to adapt your mesh.

Domain → Adapt → Refine / Coarsen...

Controls

Refinement Criterion

the criterion that Fluent uses to determine when to refine the mesh.This criterion can be based on cell

register values or an expression. Select the method using the drop-down.

Coarsening Criterion

the criterion that Fluent uses to determine when to coarsen the mesh.This criterion can be based on cell

Maximum Refinement Level

controls the number of levels of refinement used to split cells during the adaption.

Minimum Cell Volume

restricts the size of the cell that is considered for refinement. Even if the cell is marked for refinement, it

will not be refined if its cell volume is less than this threshold value.

Dynamic Adaption

enables automatic adaption, whereby Fluent automatically adapts the mesh based on the provided settings

while the solution is progressing.

Frequency (time-step | iteration)

allows you to specify the number of iterations or time steps between two consecutive automatic

mesh adaptions, depending on whether you are performing a steady-state or time-dependent solution,

and on which solver you are using.

Advanced Controls

provides additional options for advanced adaption control.

Additional Refinement Layers

allows you to specify additional cell layers for refining the mesh.

Cell Registers

drop-down list allowing you to create new cell registers and manage existing ones.

List Criteria

prints to the console the number of cells marked for refinement, the number of cells marked for

coarsening, and the number marked for both operations.

opens the

The Adaption Display Options dialog box allows you to customize the display of adaption or mask

registers. This dialog box is only available if you have used the following text command: mesh/ad-

apt/revert-to-R19.-user-interface; note that if you revert the user interface, you cannot

undo it in the current session, and some functionality is no longer available.

Domain → Adapt → More → Display Options...

Controls

Options

contains check buttons that control the drawing of the mesh and the type of graphical tool used to display

flagged cells.

Draw Mesh

toggles the ability to draw the mesh with the adaption display.This command opens the Mesh Display

Dialog Box (p. ), which allows you to select the desired surface or zone meshes to be displayed

with the markings.

Filled

toggles the solid shading of the cell wireframe.

Refine

contains options related to the display of cells marked for refinement.

Wireframe

toggles the display of the cell wireframe for cells flagged for refinement.

Marker

toggles the display of the cell marker for cells flagged for refinement.

Color

is a drop-down list of colors for the wireframe or marker for the cells marked for refinement.

Size

Marker

Color

Size

is a real number entry for the size of the refine cell marker. A symbol of size . is .% of the height

of the display screen.

Symbol

is a drop-down list of symbols that can be used for the refine cell marker.

Coarsen

Wireframe

toggles the display of the cell wireframe for cells flagged for coarsening.

Marker

toggles the display of the cell marker for cells flagged for coarsening.

Color

is a drop-down list of colors for the wireframe or marker for the cells marked for coarsening.

Size

is a real number entry for the size of the coarsen cell marker. A symbol of size . is .% of the height

Symbol

is a drop-down list of symbols that can be used for the coarsen cell marker.

The Adjacency dialog box allows you to identify, display, and rename face zones based on their adja-

cency to a selected cell zone. See Managing Adjacent Zones (p. ) for details.

Cell Zone(s)

contains a list of the cell zones for which you can find adjacent face zones.

Adjacent Face Zones

contains a list of the face zones that are adjacent to the selected cell zones.

Options

Multiple Cell Zones

allows you to select multiple cell zones at once.The zones listed in Adjacent Face Zones will be the

union of all zones adjacent to the selected cell zones.

Rename Face Zones

allows you to rename selected face zones based on adjacency or zone type.

Draw Default Mesh

brings up the Mesh Display Dialog Box (p. ) where you can specify zones of the mesh to be perman-

ently displayed as you display or hide face zones from within the Adjacency dialog box.This can be

helpful in cases where the mesh is very complex. If this option is not enabled, only the zones selected

in Adjacent Face Zones will be displayed when you click Display Face Zones.

On Selected Face Zones

contains controls for renaming face zones that are selected in Adjacent Face Zones. For details on the

renaming methods, refer to Renaming Zones Using the Adjacency Dialog Box (p. ).

renames the selected face zones incorporating the name of the adjacent cell zone and the face zone

type.

renames the selected face zones with default names based on the face zone type and, if necessary

to avoid duplicate names, the zone id.

renames the selected face zones based on a pattern match string in the From field and a replacement

string in the To field.

Abbreviate Types

uses abbreviations for the zone types when renaming rather than the full zone type text.

Exclude Custom Names

excludes from renaming any zones that do not match a recognized naming pattern.This can be

useful to prevent inadvertently replacing a meaningful name.

Displace Face Zones

displays the face zones selected in Adjacent Face Zones.

The Animation Definition dialog box allows you to specify a graphics object that will be captured

during the solution calculation so that it may be played back as an animation during postprocessing.

Controls

Name

name of the animation definition.

Record after every

specifies the frequency that images are captured during the calculation.You can select whether the fre-

quency is Iteration, Time Step (transient only) or Flow Time (transient only) from the drop-down.

Storage Type

drop-down list with the available formats for storing the animation images.

In Memory

the image files associated with the animation will lost when you exit Fluent.

PPM Image

Fluent will save the animation images in PPM Image format (.cxa), which is 2D.

HSF File

Fluent will save the animation images in HSF file format (.hsf), which is 3D.

Storage Directory

shows the location where the animation images will be stored if the Storage Type is set to PPM Image

or HSF File.

Window ID

indicates the window where the solution animation images will be displayed when the solution is calcu-

lating.

Animation View

specifies the animation object orientation that will be used when the animation images are capture during

views drop-down

list with all of the defined views.

Preview

displays the selected animation object in the graphics window specified by Window ID.

Use Active

saves the current view in the active graphics window and automatically selects it for use in the anim-

ation definition.

Animation Object

Use Active

lists the defined graphics objects that may be selected for animation.

New Object

drop-down list allowing you to create new graphics objects for animating.

Edit Object...

allows you to edit the selected graphics object.

OK

creates the animation definition and/or saves settings changes and closes the dialog box.

The Anisotropic Adaption dialog box allows you to perform anisotropic adaption for certain cell types.

See Anisotropic Adaption (p. ) for details.

Domain → Adapt → More → Anisotropic Refinement...

Controls

Cell Options

controls the marking of boundary layer cells.

Cell Distance

indicates adaption using the distance of the marked cell to the boundary zone.

Register

indicates adaption using an existing register.

Splitting Options

control how the splitting ratio is computed.

Automatic

allows the ratio to be computed automatically from the mesh.

Manual

allows you to enter a specific value for the ratio in the Split Ratio field.

Number of Cells

indicates the number of cells to be adapted and marked (available only when the Cell Distance option

Split Ratio

allows you to specify a value for the split ratio (available only when the Manual splitting option is enabled).

Registers

provides a list of existing registers (available only when the Register option is enabled).

Boundary Zones

contains a list of available boundary zones.

Refine

refines the marked cells.

The Auto Create Options dialog box allows you to define settings that you want applied to the mesh

interfaces that are created through the automatic method (for additional information, see Using a Non-

Conformal Mesh in ANSYS Fluent (p. )). It is opened by clicking the Options… button in the Unas-

signed Interface Zones group box of the Mesh Interfaces Dialog Box (p. ).

Controls

One to One Pairing

specifies that the resulting mesh interfaces have a single zone assigned to each side. Using this option

may decrease your computational expense and help with troubleshooting later on, though it may produce

a larger number of mesh interfaces for you to manage.

Interface Options

contains options related to the interface type.

Mapped

specifies that the mapped option is applied to all of the resulting interfaces for which at least one

side of the interface consists of only solid zones. Note that the mapped option will be applied regardless

of the mesh quality, and the tolerance used for mapping will be that specified in the Interface Options

Static

reduces the memory usage and processing time for interface creation (as well as for solution), especially

Static

when you are creating interfaces using many unassigned interface zones.This option will only produce

correct results if the interface zones do not move or deform relative to each other at the interfaces.

The Auto Partition Mesh dialog box allows you to set the parameters for automatic partitioning when

reading an unpartitioned mesh into the parallel solver. See Partitioning the Mesh Automatically (p. )

Controls

Method

contains a drop-down list of the recursive partition methods that can be used to create the mesh partitions.

The choices include the Cartesian Axes, Cartesian Strip, Cartesian X-Coordinate, Cartesian Y-Coordin-

ate, Cartesian Z-Coordinate, Cartesian R Axes, Cartesian RX-Coordinate, Cartesian RY-Coordinate,

Cartesian RZ-Coordinate, Cylindrical Axes, Cylindrical R-Coordinate, Cylindrical Theta-Coordinate,

Cylindrical Z-Coordinate, Metis, Polar Axes, Polar R-Coordinate, Polar Theta-Coordinate, Principal

Axes, Principal Strip, Principal X-Coordinate, Principal Y-Coordinate, Principal Z-Coordinate,

Spherical Axes, Spherical Rho-Coordinate, Spherical Theta-Coordinate, and Spherical Phi-Coordinate

techniques, which are described in Mesh Partitioning Methods (p. ).

Case File

allows you to use a valid existing partition section in a case file (that is, one where the number of partitions

in the case file divides evenly into the number of compute nodes).You need to turn off the Case File

option only if you want to change other parameters in the Auto Partition Mesh dialog box.

Across Zones

allows partitions to cross zone boundaries (the default). If turned off, it will restrict partitioning to within

each cell zone.This is recommended only when cells in different zones require significantly different

amounts of computation during the solution phase, for example if the domain contains both solid and

Optimizations

contains an option to enable pre-testing.

Pre-Test

instructs Fluent to test all coordinate directions and choose the one which yields the fewest partition

interfaces for the final bisection. Note that this option is available only when you choose Principal

Axes or Cartesian Axes as the partitioning method.

The Boundary Adaption dialog box allows you to mark or refine boundary cells on selected boundary

zones. This dialog box is only available if you have used the following text command: mesh/adapt/re-

vert-to-R19.-user-interface; note that if you revert the user interface, you cannot undo it

in the current session, and some functionality is no longer available.

Domain → Adapt → Mark/Adapt Cells → Boundary...

Controls

Options

contains three different methods for boundary adaption:

enables adaption based on a cell’s distance from the boundary, measured in number of cells.

Normal Distance

enables adaption based on a cell’s normal distance from the boundary.

Volume Distance

enables adaption based on a target boundary volume and growth factor.

Contours...

opens the Contours Dialog Box (p. ), which you can use to determine the appropriate parameters for

the boundary adaption.

Manage...

Manage...

opens the Manage Adaption Registers Dialog Box (p. ), which allows you to display and manipulate

adaption registers that are generated using the Mark command.

opens the Mesh Adaption Controls Dialog Box (p. ), which allows you to control certain aspects of the

adaption process.

sets the maximum boundary cell distance for adaption (used with the Cell Distance option.

Distance Threshold

sets the maximum normal distance for adaption (used with the Normal Distance option).

Boundary Volume

sets the boundary volume

in Equation . (p. ) (used with the Volume Distance option).

Growth Factor

sets the exponential growth factor  in Equation . (p. ) (used with the Volume Distance option).

contains a selectable list of zones on which you can refine.The boundary cells associated with the zones

that you select will be refined.

Adapt

refines the cells with edges/faces on the zones selected in the Boundary Zones list.

Mark

marks the boundary cells associated with the zones selected in the Boundary Zones list for refinement.

This command produces an adaption register.

The Cell Register Display Options dialog box allows you to customize the display of cell registers.

You can access this dialog box by clicking Display Options... in any of the cell register dialog boxes.

Controls

Options

register cells.

Draw Mesh

Controls

Options

Draw Mesh

toggles the ability to draw the mesh with the cell register display.This command opens the Mesh

Display Dialog Box (p. ), which allows you to select the desired surface or zone meshes to be dis-

played with the register cells.

Wireframe

toggles the display of the cell wireframe.

Filled

Marker

toggles the display of the cell marker.

Color

is a drop-down list of colors for the wireframe or marker for the cells.

Symbol

is a drop-down list of symbols that can be used cell marker.

Size

is a real number entry for the size of the cell marker. A symbol of size . is .% of the height of the

display screen.

The Compiled UDFs dialog box allows you to open a library of compiled user-defined functions. See

the separate Fluent Customization Manual for details.

Controls

Source Files

contains a list of source files.

Header Files

contains a list of header files.

Add...

opens the Select File dialog box.

Delete

deletes the selected file from the list.

Library Name

specifies the name of the library to be created.

Build

builds the library and compiles the user-defined function.

Load

opens the specified library and loads the user-defined function.

The Contours dialog box controls the display of contour and profile plots. See Displaying Contours

and Profiles (p. ) for details about the items below.

Controls

Contour Name

Controls

is the name for a contour plot definition.You can specify a name or use the default name  contour-id.

This control appears only for contour plot definitions.

Options

contains the check buttons that set various contour display options.

Filled

toggles between filled contours and line contours.

toggles between using scalar field values at nodes and at cell centers for computing the contours.

When the Filled option is off, Node Values is always on. See Choosing Node or Cell Values (p. )

Contour Lines

combines filled contours with line contours.This option is only available when both the Filled and

Node Values options are enabled.

toggles between basing the minimum and maximum values on the range of values on the selected

surfaces (off), and basing them on the range of values in the entire domain (on, the default).

Auto Range

toggles between automatic and manual setting of the contour range. Any time you change the

Contours of selection, Auto Range is reset to on.

determines whether or not values outside the prescribed Min/ Max range are contoured when using

Filled contours. If selected, values outside the range will not be contoured. If not selected, values

below the Min value will be colored with the lowest color on the color scale, and values above the

Max value will be colored with the highest color on the color scale. See Specifying the Range of

Magnitudes Displayed (p. ) for details.

Draw Profiles

causes the addition of a profile plot to the contour plot.The Profile Options Dialog Box (p. ) is

opened when Draw Profiles is selected.

Draw Mesh

Draw Mesh

toggles between displaying and not displaying the mesh.The Mesh Display Dialog Box (p. ) is

opened when Draw Mesh is selected.

Coloring

specifies how the contours appear.

Banded

the contour coloring features distinct color bands corresponding to the colormap.

Smooth

the contours feature a smooth transition between colors.

Colormap Options...

opens the Colormap Dialog Box (p. ), allowing you to customize the colormap for this graphics object.

Contours of

contains a list from which you can select the scalar field to be contoured.

Min

shows the minimum value of the scalar field. If Auto Range is off, you can set the minimum by typing a

new value.

Max

shows the maximum value of the scalar field. If Auto Range is off, you can set the maximum by typing a

new value.

Surfaces

contains a list from which you can select the surfaces on which to draw contours. For 2D cases, if no surface

is selected, contouring is done on the entire domain. For 3D cases, you must always select at least one

surface.

Point

Line/Rake

Plane

Quadric

Iso-Clip

Display

draws the contours in the active graphics window.

Compute

Iso-Clip

Display

Compute

calculates the scalar field and updates the Min and Max values (even when Auto Range is off).

plots the contour in the active graphics window and saves the contour plot definition.This button appears

only for contour plot definitions and replaces the Display button.

The convergence conditions facility allows you to set convergence conditions on the solution based

on the values from report definitions (surface, volume, lift, drag, and so on). See Convergence Condi-

tions (p. ) for details on setting up the Convergence Conditions dialog box.

Note

If you are solving a transient case, the Convergence Conditions dialog box will relabel

some fields since the transient case uses time-steps rather than iterations. These alternate

labels are indicated below.

Solution → Reports → Conditions...

Controls

Active

check box for deactivating/activating individual convergence conditions.

name of the convergence condition.

Report Definition

name of the report definition used in judging convergence.

Stop Criterion

specifies the criterion below which the solution is considered to be converged.

Ignore Iterations Before | Ignore Time Steps Before

ignores the first few iterations/time-steps if you expect the solution to fluctuate initially.

Use Iterations | Use Time Steps

specifies the number of previous iterations/time-steps to be included in the report definition conver-

gence check.

Check For

Check For

specify whether Fluent checks for convergence at every time step or every iteration.

Solution Convergence

Time Step Convergence

Choose Condition

to select the convergence conditions.

All Conditions are Met

The solution is considered to be converged if all of the convergence conditions’ criteria are sat-

isfied, including those in the Residual Monitors Dialog Box (p. ).

Any Condition is Met

The solution is considered to be converged if any of the convergence conditions’ criteria is satis-

fied, including those in the Residual Monitors Dialog Box (p. ).

Every Iteration | Every Time-Step

to select how often convergence checks are done.

The Create/Edit Mesh Interfaces dialog box allows you to manually create mesh interfaces for use

with sliding meshes (see Using Sliding Meshes (p. )) or multiple reference frames (see Mesh Setup

for a Multiple Moving Reference Frame (p. )), or for meshes with non-conformal boundaries (see

Non-Conformal Meshes (p. )). This dialog box requires you to decide which interface zones make

up both sides of each mesh interface. While it is possible to create every type of mesh interface using

this dialog box, it is only necessary when you want your interface to use the periodic or periodic repeats

option; for all other types it is more convenient to automatically create interfaces using the Mesh In-

terfaces Dialog Box (p. ), especially when you have many interface zones and/or are unfamiliar with

their names / locations. For details, see Using a Non-Conformal Mesh in ANSYS Fluent (p. ).

The Create/Edit Mesh Interfaces dialog box is opened by clicking the Manual Create... button in the

Mesh Interfaces Dialog Box (p. ).

Controls

Mesh Interface

contains a text entry box in which you can set the name of the mesh interface, and a list from which you

can select an existing mesh interface.

Interface Zones Side , Interface Zones Side

contain selectable lists for the interface zones that make up the mesh interface and informational fields

that show the names of the zones you selected in each list. (You cannot edit the top fields; the names in

these fields will be the names of the zones you selected in the list below it.)

Periodic Boundary Condition

allows you to create a non-conformal periodic boundary condition interface.

should be enabled when each of the two cell zones has a single pair of conformal or non-conformal

periodics adjacent to the interface.This option is typically used in conjunction with the sliding mesh

model, when simulating the interface between a rotor and stator; it allows ANSYS Fluent to treat the

interface between the sliding and non-sliding zones as periodic where the two zones do not overlap.

For details, see The Periodic Repeats Option (p. ).

Coupled Wall

allows you to specify that the interface acts as a thermally coupled wall.

Matching

is relevant if only interface internal zones should be created (that is, interior or wall / shadow pairs),

Matching

since the interface zones on both sides are aligned.With the Matching option, even interface zones

that are not perfectly aligned are treated as if they are; however, if the discrepancy between the inter-

face zones on both sides exceeds default thresholds, then warning messages will be displayed. Note

that the Matching option is compatible with the Periodic Boundary Condition, Coupled Wall, and

Static options. For more information about the recommended uses of this option, see Matching Op-

tion (p. ).

Mapped

enables an alternative approach for modeling coupled walls between zones. This approach is

more robust than the standard non-conformal interface formulations when the interface zones

penetrate each other or have gaps between them. It requires that at least one side of the in-

terface consists of only solid zones.

Note

Static

reduces the memory usage and processing time (for interface creation and solution), especially

when there are many zones on both sides of the interface. This option will only produce correct

results if the interface zones do not move or deform relative to each other at the interface,

and it is not compatible with the Periodic Boundary Condition, Periodic Repeats, or Mapped

options.

Non-Overlapping Zones Side , Non-Overlapping Zones Side

display the names of any wall boundary zones created by ANSYS Fluent during the process of creating

the selected mesh interface. If the two interface zones overlap each other completely, then the wall

boundaries are created but with zero faces.

Interface Wall Zones Side , Interface Wall Zones Side

display the names of any wall interface zones created by ANSYS Fluent during the process of creating

the selected mesh interface.

Interface Interior Zones

displays the names of any interface interior zones created by ANSYS Fluent during the process of creating

the selected mesh interface.This is used for embedded LES, when there is a need to be able to convert

an interior zone into a RANS-LES interface.

Type

allows you to select a periodicity that is either Translational or Rotational.

Offset

is the offset coordinates or angle, depending on whether Translational or Rotational periodicity is

selected. Note that when Auto Compute Offset is enabled, the Offset fields are not editable.

Auto Compute Offset

will result in ANSYS Fluent finding the offset. If this option is disabled, then you will have to provide

the offset coordinates or angle in the required fields, depending on whether Translational or Rota-

tional periodicity is selected.

Mapped

Enable Local Tolerance

(when enabled) allows you to overwrite any value specified in the Tolerance group box in the Interface

Options Dialog Box (p. ), and is used on the selected interface only.

Local Edge Length Factor

(when enabled) allows you to specify the multiplier that Fluent uses with the smallest edge length

of the interface zones to calculate the tolerance for mapping. Disabling Local Edge Length Factor

allows you to specify an absolute value for the tolerance.

performs one of the following:

If you have entered a new Mesh Interface name and selected unassigned zones from the Interface

Zones Side  and Interface Zones Side  selection lists, a new mesh interface is created.

If you have made a selection from the Mesh Interface list, the Edit Mesh Interfaces Dialog Box (p. )

will open so that you can revise the settings of existing mesh interfaces.

Delete

deletes the mesh interface selected under Mesh Interface.

Draw

allows you to display interface zones or mesh interfaces in the graphics window. Note that you can only

select and display an interface zone from Interface Zones Side  or Interface Zones Side  if it is not

yet assigned to an existing mesh interface. After a Mesh Interface is created, you can select the appropriate

mesh interface and click the Draw button to display all of the zones under Interface Zones Side  and

Interface Zones Side .

List

prints information about the selected Mesh Interface in the console.When you click this button, ANSYS

Fluent will list the two interface boundaries and (if you have initialized the solution) all new zones that

were created (that is, wall and/or interior zones).

The Custom Field Function Calculator dialog box allows you to define custom field functions based

on existing functions, using simple calculator operators. Any functions that you define will be added

to the list of default flow variables and other field functions provided by ANSYS Fluent.

Important

Important

See Creating a Custom Field Function (p. ) for details about the items below.

Controls

displays the function that you are currently defining. As you select each item from the Field Functions

list or the calculator keypad, it will appear in the Definition text entry box.You cannot edit the contents

of this box directly; if you want to delete part of a function, use the Delete button on the keypad.

(Calculator Buttons)

are buttons that perform calculator operations.When you select a calculator button (by clicking on it),

the appropriate symbol will appear in the Definition text entry box.

Select Operand Field Functions from

contains the available field functions and the means for selecting them.

Field Functions

contains a list from which you can select a variable to be used in the definition of a new function.

Select

enters the variable that is currently selected in the Field Functions list in the Definition field.

New Function Name

specifies the name of the function you are defining. Should you decide to change the function name after

you have defined the function, you can do so in the Field Function Definitions Dialog Box (p. ), which

you can open by clicking on the Manage... button.

Define

creates the function and adds it to the list of Custom Field Functions within the drop-down list of

available field functions.The Define button is grayed out after you create a new function or if the

Definition field is empty.

Manage...

opens the Field Function Definitions Dialog Box (p. ), which enables you to check, rename, save, load,

and delete custom field functions.

Manage...

The Custom Laws dialog box is used to incorporate user-defined functions (see the separate Fluent

Customization Manual for details) in place of the default physical laws ( through ) used in the

heat/mass transfer calculations.

The Custom Laws dialog box is opened from the Set Injection Properties Dialog Box (p. ).

Controls

First Law, Second Law,Third Law, Fourth Law, Fifth Law, Sixth Law

contain drop-down lists in which you can choose a user-defined particle law to replace the standard law.

Switching

contains a drop-down list in which you can select a user-defined function that customizes the way ANSYS

Fluent switches between particle laws.

The Deactivate Cell Zones dialog box allows you to deactivate a single cell zone or multiple zones.

See Deactivating Zones (p. ) for details.

Controls

Cell Zones

contains a list of cell zones from which you can select the zone to be deactivated.

Deactivate

deactivates the selected cell zones.

The Define Control Points dialog box allows you to create, modify, and delete control points for the

mesh morpher/optimizer when the unstructured control point distribution is selected. See Using the

Mesh Morpher/Optimizer (p. ) for details about using this dialog box.

The Define Control Points dialog box is opened from the Mesh Morpher/Optimizer Dialog Box (p. ).

Controls

Control Points

Controls

lists the control points you have created and allows you to modify and delete them.

Definition Tools

provides tools for defining the control points.

Mouse-Probe

allows you to create control points by probing (using the right mouse button, by default) in the

Distribute Throughout Zone

allows you to quickly create a number of control points and distribute them on mesh nodes

throughout a specific boundary zone.

Zones

allows you to select the boundary zone throughout which you want to distribute control points.

Approximate Number

allows you to specify the approximate number of control points you want to distribute throughout

a zone. Note that due to the method by which the control points are distributed, the actual

number may exceed the value you enter.

Distribute

creates a number of control points on mesh nodes throughout the specified zone (within the

bounding box) with a distribution that is based on the distribution of the cell faces in that zone.

Coordinates

allows you to view and modify the coordinates of control points, as well as to create new control

points and to delete existing control points.

X, Y, Z

displays the coordinates of the selected Control Point, and allows you to define new ones and

edit existing ones.

Create

creates a new control point at the currently displayed X, Y, and Z coordinates.

Modify

revises the X, Y, and Z coordinates of the selected Control Point.

Delete

deletes the selected Control Point.

Modify

Delete

The Delete Cell Zones dialog box allows you to delete a single cell zone or multiple zones. See Deleting

Controls

Cell Zones

contains a list of cell zones from which you can select the zone to be deleted.

Delete

deletes the selected cell zones.

The Display Options - Adaption dialog box allows you to customize how the cells marked for adaption

are displayed.

This dialog box is accessed by clicking Display Options in the Adaption Controls Dialog Box (p. ).

Controls

Options

contains check boxes that controls the drawing of the mesh.

Draw Mesh

Refinement Cells

Faces

controls whether cell faces are displayed on the cells marked for refinement.

Edges

controls whether cell edges are displayed on the cells marked for refinement.

Centroid

controls whether the cell centroid is displayed on the cells marked for refinement.

Face Color

controls the color of the cell faces on the cells marked for refinement.

Edge Color

controls the color of the cell edges on the cells marked for refinement.

Edge Width

controls the thickness of the cell edges on the cells marked for refinement.

Coarsening Cells

Edge Width

contains options related to the display of cells marked for coarsening.

Faces

controls whether cell faces are displayed on the cells marked for coarsening.

Edges

controls whether cell edges are displayed on the cells marked for coarsening.

Centroid

controls whether the cell centroid is displayed on the cells marked for coarsening.

Face Color

controls the color of the cell faces on the cells marked for coarsening.

Edge Color

controls the color of the cell edges on the cells marked for coarsening.

Edge Width

controls the thickness of the cell edges on the cells marked for coarsening.

Common Cells

contains options related to the display of cells marked for both refinement and coarsening.

Faces

controls whether cell faces are displayed on the cells marked for both refinement and coarsening.

Edges

controls whether cell edges are displayed on the cells marked for both refinement and coarsening.

Centroid

controls whether the cell centroid is displayed on the cells marked for both refinement and coarsening.

Face Color

controls the color of the cell faces on the cells marked for both refinement and coarsening.

Edge Color

controls the color of the cell edges on the cells marked for both refinement and coarsening.

Edge Width

controls the thickness of the cell edges on the cells marked for both refinement and coarsening.

Controls

Average Over

(optional) To have Fluent calculate a running average for the DPM Report Definition you can enter a

Controls

positive integer greater than  (the default) for Average Over.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the

same units as the other report definitions included in the selected report plot).

Create

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

prints the value of the report definition to the console.

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-

op.

Output Quantity

Injected Mass

(unsteady particle tracking only) reports the total DPM mass injected into the domain.

Mass in Domain

(unsteady particle tracking only) reports the total DPM mass present in the domain.

Mass in Fluid

(unsteady particle tracking only) reports all DPM mass currently residing as free-stream particles in

the domain.This option is available only with the wall-film DPM boundary condition.

Mass in Film

(unsteady particle tracking only) reports all DPM mass currently residing in Lagrangian wall-film.This

option is available only with the wall-film DPM boundary condition.

Escaped Mass

reports the DPM mass that has left the domain through a certain boundary or boundaries.

Evaporated Mass

reports the total evaporated DPM mass for the selected injection(s).The quantity accounts for fully

evaporated particles as well as all mass that has evaporated from any other particles. For unsteady

tracking, this includes particles that are still present in the domain.

Penetration Length

(unsteady particle tracking only) reports the total penetration length in meters.

lists the injections that you can select for discrete phase reporting. For the Escaped Mass output quantity,

this item is available only if you have enabled the report/dpm-zone-summaries-per-injection

text command. Note that for unsteady particle tracking, if you want to report the mass of escaped particles

per injection, this text command must be enabled before any particles are injected into the domain.

contains a selectable list of valid boundary zones for escaped mass reporting.

Show Mass Flow/Change Rate

(unsteady particle tracking only) if enabled, specifies that the mass flow rate will be reported (default).

Otherwise the total mass will be reported.This item is not available for the Penetration Length report.

Particles Mass Fraction

the mass fraction expected between the injection nozzle and the penetration length.This item is available

only for the Penetration Length reports.

User-Specified Origin and Direction

once enabled, it allows you to specify the Origin and Direction of the selected injection(s).This item is

available only for the Penetration Length reports.

OK

creates the report definition.

Compute

computes the value of the report definition and prints to the console.

Solution → Reports → Definitions → New → Flux Report → DPM Mass Source | DPM Enthalpy

Source | DPM Sensible Enthapy Source

Controls

Function

reports the mass contributions from the particle injections.

reports the heat contributions from the particle injections.

reports the sensible heat contributions from the particle injections.

(optional) To have Fluent calculate a running average for the DPM Source Report Definition you can

enter a positive integer greater than  (the default) for Average Over.

op.

Create

Frequency

Compute

OK

Solution → Reports → Definitions → New → Force Report → Drag...

Controls

Options

Per Zone

specifies whether or not the drag for multiple walls zones should be monitored on each wall zone

separately.When this option is turned off (the default), Fluent computes and monitors the total drag

for all of the selected walls zones combined together.

Average Over (Time-Steps), Average Over (Iterations)

(optional) To have Fluent calculate a running average for the Drag Report Definition you can enter

is your specified Av-

erage Over value. When the iteration/time step number is lower than

, Fluent calculates the av-

erage of the available variable values.

Force Vector

contains the components of the force vector.

X,Y,Z

Create

Frequency

op.

Report Output Type

specifies the report definition as a unitless quantity.

Drag Force

specifies that the report definition has units of force.

Wall Zones

lists the zones you can select for drag coefficient or drag force computation.

OK

Compute

computes the value of the report definition at the selected zone(s) and prints to the console.

OK

Compute

The DTRM Graphics dialog box allows you to display rays and clusters used by the DTRM. See Displaying

Rays and Clusters for the DTRM (p. ) for details.

Controls

contains options for the different items you can display.

Cluster

specifies the display of clusters.

Ray

specifies the display of rays.

Options

contains check buttons that control display options.

Draw Mesh

Cluster Type

specifies whether Surface clusters or Volume clusters are to be displayed.This section of the dialog box

appears when Cluster is selected as the Display Type.

Cluster Selection

contains options for cluster displays.This section of the dialog box appears when Cluster is selected as

the Display Type.

Display All Clusters

enables the display of all surface or volume clusters in the domain.

Ray Parameters

contains controls for displaying rays.This section of the dialog box appears when Ray is selected as the

Display Type.

control the number of rays being traced. (See Controlling the Rays (p. ).)

Nearest Point

specifies a point (X,Y,Z) near the cluster to be displayed (or the cluster from which the rays should start).

The Nearest Point controls are not available when Display All Clusters is selected under Cluster

Selection.

Select Point With Mouse

is an alternative method for specifying the Nearest Point using your mouse, by clicking the button.

Display

displays the specified cluster(s) or rays.

The DTRM Rays dialog box allows you to define the rays used by the discrete transfer radiation

model (DTRM). It opens automatically when you click OK after selecting the Discrete Transfer model

in the Radiation Model Dialog Box (p. ). See Setting Up the DTRM (p. ) for details about the items

below.

Physics → Model Specific → DTRM Rays...

Controls

contains parameters for the clusters (see Clustering in the Theory Guide).

Cells Per Volume Cluster, Faces Per Surface Cluster

control the number of radiating surfaces and absorbing cells. (See the explanation in Controlling the

Clusters (p. ).)

contains parameters for the ray traces (see Ray Tracing in the Theory Guide).

control the number of rays being traced. (Guidelines are provided in Controlling the Rays (p. ).)

Display Clusters

generates a graphical display of the clusters in the domain. (This item is available only after you have

created or read a ray file.)

The Edit Mesh Interfaces dialog box allows you to edit existing mesh interfaces (see Using a Non-

Conformal Mesh in ANSYS Fluent (p. )). It is opened by making a selection from the Mesh Interfaces

list in the Mesh Interfaces Dialog Box (p. ) and clicking Edit....

Controls

Mesh Interfaces

allows you to select the mesh interfaces you would like to edit. Note that you can click the

button

Controls

button

to group the interfaces in the list by their currently enabled interface option(s), which allows you to select

/ deselect all those of a particular type by simply clicking the top-level branch.

edits the name of the mesh interface.This is only available when a single interface is selected.

contains options related to the interface type.These options can be applied when a single or multiple

interfaces are selected.

Matching

tion (p. ).

Mapped

Note

Static

options.

Periodic Boundary Conditions

Type

Offset

Mapped

Mapped

Options Dialog Box (p. ), and is applied to the selected interface only.

Interface Zones

highlights the list of interface zones that make up the selected mesh interface and allows you to edit the

list (provided that the zones you select are unassigned and located appropriately).This functionality is

only available when a single interface is selected.

List

prints information in the console about the first mesh interface you selected.When you click this button,

ANSYS Fluent will list the two interface boundaries and (if you have initialized the solution) all new zones

that were created (that is, wall and/or interior zones).

Apply

saves the revised settings for the selected mesh interfaces.

Solution → Reports → File...

Select a report file in the Report File Definition dialog box and click Edit... to open the Edit Report

File dialog box.

Controls

Name

editable field displaying the name of the report file.

Active

check box (enabled by default) that determines if the file is written during the solution calculation.

Available Report Definitions

lists all of the existing report definitions not currently part of this report file.

Add>>

Add>>

moves the selected report definition(s) to the Selected Report Definitions list.

<<Remove

moves the selected report definition(s) to the Available Report Definitions list.

File Name

allows you to specify the name used when the file is saved.

Browse...

opens the Select File dialog box, allowing you to specify the location where the report file will be saved.

Full File Name

displays the name and location of the report file once it has been saved.

Get Data Every

indicates the frequency that the report definition data is written to the file.The default value of  allows

you to write to the file at every iteration or time-step. If you select flow-time, then you must specify the

frequency for writing the file units of time.Time-step and flow-time are only a valid choices when you

are calculating unsteady flow.

indicates whether or not the contents of the report file are printed to the console at the frequency specified

in the Get Data Every field.

Selected Report Definitions

lists all of the existing report definitions currently included in this report file.

New

drop-down list allowing you to create new report definitions (surface, volume, force, flux, dpm, and user-

defined).

Edit...

allows you to modify the highlighted report definition in the Selected Report Definition list.

Solution → Reports → Plot...

Select a report plot in the Report Plot Definition dialog box and click Edit... to open the Edit Report

Plot dialog box.

Controls

Name

editable field displaying the name of the report plot.

Active

Controls

Name

Active

check box (enabled by default) that determines if the plot is plotted during the solution calculation.

lists all of the existing report definitions not currently part of this report plot.

Add>>

<<Remove

Options

Plot Window

allows you to specify the graphics window for this report plot.

Curves...

opens the Curves Dialog Box (p. ).

Axes...

opens the Axes Dialog Box (p. ).

indicates the frequency that the report definition data is plotted.The default value of  allows you to

write to the file at every iteration or time-step. If you select flow-time, then you must specify the frequency

for plotting the data in units of time.Time-step and flow-time are only a valid choices when you are cal-

culating unsteady flow.

Plot Title

provide a title for the plot.

X-Axis Label

choose whether the X-axis is flow-time or time-step.

Y-Axis Label

enter a label for the Y-axis.

indicates whether or not the contents of the report plot are printed to the console at the frequency spe-

cified in the Get Data Every field.

lists all of the existing report definitions currently included in this report plot.

New

defined).

Edit...

defined).

Edit...

The Execute on Demand dialog box allows you to run a specified user-defined function immediately.

See the separate Fluent Customization Manual for details.

Controls

Execute on Demand

selects the user-defined function to be run.

Execute

runs the selected function.

New...

Controls

Name

an editable field allowing you to name the expression. The Name field is not editable when the expression

is in use.

displays the formula of the expression as you create it.

(Optional) allows you to provide more of a description of this expression beyond the name.

Used In

lists the locations where the expression is used.

Use as parameter

allows you to define the expression as an input parameter.

Drop-downs

The items in these drop-downs may be used in creating named expressions.

Functions

lists the available functions (conditional, mathematical, and so on) that are available for constructing your

expression.

Variables

lists all of the supported variables.

lists the defined cell registers.

Constants

lists the available pre-defined constants.

Expressions

lists the defined expressions.

Report Definitions

lists the defined report definitions.

For additional information on expressions, refer to Fluent Expressions Language (p. ).

Solution → Reports → Definitions → New → Expression...

Controls

Name

Controls

Name

is in use.

(optional) To have Fluent calculate a running average for the Expression Report Definition you can

Create

Frequency

op.

Compute

op.

Compute

prints the value of the expression report definition to the Console.

The items in these drop-downs may be used in creating expression report definitions.

Functions

Variables

Constants

For additional information on expression report definitions, refer to Expression Report Definition (p. ).

The Field Function Definitions dialog box allows you to check, rename, save, load, and delete custom

field functions that you defined in the Custom Field Function Calculator Dialog Box (p. ). See Manip-

ulating, Saving, and Loading Custom Field Functions (p. ) for details about the items below.

The Field Function Definitions dialog box is opened from the Custom Field Function Calculator Dialog

Box (p. ).

Controls

displays the function selected in the Field Functions list.This display is for informational purposes only;

you cannot edit it.

contains a selectable list of custom field functions.When you select a function, its definition will appear

in the Definition box and its name will appear in the Name text entry box.

Name

Name

displays the name of the currently selected field function.You can enter a new name in this box if you

want to rename the function.

ID

reports the ID number of the selected function.The field function at the top of the list has an ID of , the

second function has an ID of , and so on.

Rename

changes the name of the selected function to the name specified in the Name text entry box.

Delete

deletes the selected field function.

Save...

opens The Select File Dialog Box (p. ), where you can specify a file in which to save all of the functions

in the Field Functions list.

Load...

opens the Select File dialog box, where you can specify a file from which to read custom field functions

(that is, a file that you saved using the Save... button above).

Controls

Options

Phase

Per Zone

specifies whether or not the chosen field variable is calculated from all of the selected boundary zones

combined (default) or individually on each of the selected boundary zones.

(optional) To have Fluent calculate a running average for the Flux Report Definition you can enter a

Create

Frequency

op.

selects the integration method used on the selected cell zones.The available report types are the same

as those in the Volume Integrals Dialog Box (p. ). See Volume Integration (p. ) for details.

OK

Compute

Solution → Reports → Definitions → New → Force Report → Force...

Controls

Options

Per Zone

specifies whether or not the force for multiple walls zones should be monitored on each wall zone

separately.When this option is turned off (the default), Fluent computes and monitors the total force

(optional) To have Fluent calculate a running average for the Force Report Definition you can enter

X,Y,Z

Create

Frequency

op.

Wall Zones

lists the zones you can select for force computation.

OK

Compute

op.

Wall Zones

OK

Compute

The Fuse Face Zones dialog box allows you to fuse boundaries (that is, remove duplicate nodes and

faces and delete artificial internal boundaries) created by assembling multiple mesh regions. (See

Reading Multiple Mesh/Case/Data Files (p. ) for details on importing such meshes.) See Fusing Face

Zones (p. ) for information about using this dialog box.

Domain → Zones → Combine... → Fuse...

Controls

Zones

contains a list of face zones from which you can select the boundaries to be fused.

Use default name for new fused zone

specifies whether to use an automatically generated default name for the fused zone.

Fused zone name

specifies the desired name for the fused zone if Use default name for new fused zone is disabled.

Tolerance

is a fraction of the minimum edge length of the face, used to determine whether or not nodes are coin-

cident. If all of the appropriate faces do not get fused using the default Tolerance, you should increase

it and attempt to fuse the zones again.The Tolerance should not exceed ., or you may fuse the wrong

nodes.

Fuse

fuses the selected zones. It is enabled only when you have selected a minimum of two zones.

The Geometry Based Adaption Controls dialog box allows you to set projections. See Performing

Geometry-Based Adaption (p. ) for details about the items below.

The Geometry Based Adaption Controls dialog box is opened from the Geometry Based Adaption

Controls

Controls

contains parameters to define geometry based adaption.

Disable Geometry Based Adaption for this Zone

disables the geometry reconstruction for selected zones in the domain.

Levels of Projection Propagation

is the number of layers of the nodes you want to project.

Direction of Projection

allows you to specify the direction in which you want to project the nodes.

Background Mesh

allows you to load the surface mesh as a background mesh for adaption.

The Geometry Based Adaption dialog box allows you to reconstruct the geometry while performing

boundary adaption. See Geometry-Based Adaption (p. ) for details.

Controls

Reconstruct Geometry

enables geometry based adaption parameters.

Surface Meshes...

opens the Surface Meshes Dialog Box (p. ).

Wall Zones

allows you to select the wall zones you want to adapt.

Set...

opens the Geometry Based Adaption Controls Dialog Box (p. ).

The Gradient Adaption dialog box allows you to mark or adapt to gradients of a specified field variable.

This dialog box is only available if you have used the following text command: mesh/adapt/revert-

to-R19.-user-interface; note that if you revert the user interface, you cannot undo it in the

current session, and some functionality is no longer available.

Domain → Adapt → Mark/Adapt Cells → Gradient...

Controls

Options

Controls

Options

contains the check buttons that toggle the ability to mark and/or adapt cells for refinement or coarsening.

Refine

toggles the ability to refine or mark cells for refinement.

Coarsen

toggles the ability to coarsen or mark cells for coarsening (available in 2D and axisymmetric cases).

Normalize per Zone

toggles the ability of zonal normalization.

opens the Contours Dialog Box (p. ), which you can use as an aid to selecting adaption thresholds by

displaying contours of adaption function.

Manage...

Method

contains options for specifying the criterion for adaption.

Curvature

specifies the use of the second gradient of a field variable for adaption.This approach is recommended

for problems with smooth solutions.

Gradient

specifies the use of the first gradient of a field variable for adaption.This approach is recommended

for problems with strong shocks.

Iso-Value

allows you to customize the adaption criterion (using custom field functions, user-defined scalars,

and so on).

Normalization

contains the options available for normalization.

Standard

specifies that the gradient or curvature is not normalized.

Scale

specifies that the gradient or curvature is scaled by its average value in the domain.

Normalize

Standard

Scale

Normalize

specifies that the gradient or curvature is scaled by its maximum value in the domain (that is, the

gradient or curvature is bounded by [, ]).

Dynamic

contains options to specify dynamic gradient adaption.

Dynamic

enables dynamic gradient adaption.

Interval

allows you to specify the number of iterations or time-steps between two consecutive automatic

mesh adaptions, depending on whether you are performing a steady-state or a time-dependent

solution, and on which solver you are using.

Gradients of

contains a list of the field variables that can be used in the gradient adaption function.

Min/Max

displays the minimum and maximum cell values of the gradient adaption function based on the selected

quantity.

Coarsen Threshold

designates the threshold values for coarsening the mesh. Cells with adaption function values below the

Coarsen Threshold will be marked for coarsening.

Refine Threshold

designates the threshold values for refining the mesh. Cells with adaption function values above the Refine

Threshold will be marked for refinement.

Adapt

adapts the mesh based on the gradients of the selected scalar quantity, the coarsening and refining

toggle buttons and thresholds, and the adaption limits.

Mark

marks cells to be refined and/or coarsened based on the gradients of the selected quantity and the

coarsening and refining toggle buttons and thresholds.This command produces an adaption register.

Compute

computes the minimum and maximum cell values of the gradient adaption function with the selected

Compute

scalar quantity.The values are displayed in the Min and Max real number fields.

The Import Particle Data dialog box allows you to import particle history data for display purposes.

See Importing Particle Data (p. ) for details.

Controls

Options

contains the check buttons that set various import particle data options.

Auto Range

toggles between automatic and manual setting of the particle data range.

Draw Mesh

Style

allows you to select pathline style.

Attributes...

opens the Path Style Attributes Dialog Box (p. ).This allows you to modify the line width, cylinder radius

or marker size.

Color by

contains a list from which you can select the scalar field to be used to color the particle data.

Min,Max

allows you to set the range when Auto Range is disabled.

Steps

sets the maximum number of steps a particle can advance.

Skip

allows you to “thin out” the pathlines.

Display

displays pathlines.

Pulse

animates the particle positions.The Pulse button will become the Stop ! button during the animation,

and you must click Stop ! to stop the pulsing.

Read...

opens a file selection dialog box where you can enter a file name and a directory for the imported data.

The Imprint Surface dialog box allows you to define a surface on top of an existing cell zone for

postprocessing purposes. See Imprint Surfaces (p. ) for details about the following items.

Controls

Imported Surface

lists the surfaces that you have imported.

Read...

opens The Select File Dialog Box (p. ), so that you can select surface files for import.

Display

allows you to display the selected surfaces.

Manage...

opens the Surfaces Dialog Box (p. ), where you can rename and delete surfaces and determine

their sizes.

New Surface Name

designates the name of the new surface.The default name format is <original-name>(imprint)-

<id>.

From Zones

allows you to select the zones where you want to import/imprint the surface mesh.

Note

If no zone is selected, then the entire domain is considered.

Create

creates the new surface, imprinted with the mesh of the selected cell zone.

The Improve Mesh dialog box controls the quality-based smoothing of the numerical mesh. See Im-

proving the Mesh by Smoothing and Swapping (p. ) for details about the items below.

Domain → Mesh → Improve...

Controls

Percentage of Cells to be Improved

sets the percentage of the total cells on which improvements are attempted. Note that the cells selected

for improvement are in the areas of the mesh that exhibit the lowest orthogonal quality.

defines the number of successive smoothing sweeps performed on the mesh.

Improve

initiates the desired number of smoothing iterations.

The Injections dialog box allows you to create, delete, and list discrete phase injections, and access

Improve

the Set Injection Properties Dialog Box (p. ) and the Set Multiple Injection Properties Dialog

Box (p. ), in which you can set the properties for the injections. See Creating and Modifying Injec-

Physics → Model Specific → Discrete Phase → Injections...

Controls

contains a list from which you can select one or more injections in order to set, copy, or modify properties,

or delete or list injections.

Create

creates a new injection and opens the Set Injection Properties Dialog Box (p. ), in which you can set

its properties.

Copy

creates a new injection with the same properties as the selected injection and opens the Set Injection

Properties Dialog Box (p. ) where the new injection’s properties can be modified.

Delete

deletes the injection(s) selected in the Injections list.

List

lists the initial conditions for the particle streams in the injection(s) selected in the Injections list.

Read...

opens The Select File Dialog Box (p. ) where you will select the injection file to read in.

Write...

allows you to select the injection from the list and write it to a file.

Set...

opens the Set Injection Properties Dialog Box (p. ) for the injection selected in the Injections list or

the Set Multiple Injection Properties Dialog Box (p. ) if more than one injection is selected in the Injec-

tions list.

The Input Summary dialog box allows you to report the current settings for physical models, boundary

conditions, material properties, and solution parameters. See Generating a Summary Report (p. )

for details about the items below.

Controls

Report Options

contains a selectable list of the information that is available for the report.

Print

prints the selected information to the console.

Save...

opens The Select File Dialog Box (p. ), in which you can specify the filename under which to save the

output of the summary report.

The Interface Options dialog box allows you to update which mesh interfaces use the mapped option

and the related settings (see The Mapped Option (p. ) for additional information). It is opened by

clicking the Options… button in the Mesh Interfaces group box of the Mesh Interfaces Dialog

Box (p. ).

Controls

Mapped Interface

contains options related to mapped interface specification.

Auto (Tolerance-Based)

specifies that all mesh interfaces that have interface zones that penetrate each other are

automatically defined as Mapped interfaces (provided that at least one side of each interface

consists only of solid zones).

Tolerance

(when enabled) allows you to specify the multiplier that Fluent uses with the smallest edge

length of the interface zones to calculate the tolerance for mapping. Disabling Local Edge

Length Factor allows you to specify an absolute value for the tolerance. Note that this does

not overwrite any locally specified tolerance in the Edit Mesh Interfaces dialog box.

Solution Controls

Mapping Frequency

specifies how often calculation values are interpolated across mapped interfaces.

allows you to reduce the rate of change per iteration of physical quantities across mapped interfaces

to aid with convergence. For additional information on setting under-relaxation factors, see Setting

Update

applies the selection(s) made in the Interface Options dialog box.This button is grayed out until you

make a selection in the Mapped Interface or Tolerance group boxes; it also returns to being grayed out

once it is clicked.

Note

Selecting Auto or Enforced and clicking Update applies these selections globally for all

relevant interfaces. Once you click Update you can return to the Mesh Interfaces dialog

box to modify local settings for individual interfaces.

The Interpreted UDFs dialog box allows you to compile user-defined functions. See the separate

Fluent Customization Manual for details.

User Defined → User Defined → Functions → Interpreted...

Controls

Source File Name

sets the name of your user-defined function.

CPP Command Name

sets the name of your C preprocessor.

Stack Size

sets the size of the stack. Keep the default Stack Size setting of , unless the number of local variables

in your function will cause the stack to overflow. In this case, set the Stack Size to a number that is

greater than the number of local variables used.

Display Assembly Listing

indicates whether or not to display a listing of assembly language code in your console window as the

function compiles.

Use Contributed CPP

specifies the use of the C preprocessor that ANSYS Fluent has supplied, instead of your own.

Interpret

interprets the specified function.

The Iso-Clip dialog box allows you to interactively clip surfaces. The clipped surface consists of those

points on the selected surface where the scalar field values are within the specified range. See Clipping

Surfaces (p. ) for details about the items below.

Controls

Clip to Values of

contains a list from which you can select the scalar field to be used for clipping.

Phase

allows you to select the phase when one of the multiphase models is selected in the Multiphase Model

Min, Max

set the minimum and maximum values in the clipping range.There are two ways you can set the Min

and Max:

You can set a value interactively by moving the indicator in the dial above the Min or Max field with

the left mouse button.This will also create a temporary surface in the graphics window. Using the dial

allows you to preview the clipped surfaces before defining them. Note: Even though the clipped surface

is displayed, it is only a temporary surface.To clip the surface, use the Clip button after deciding on

the minimum and maximum values.

You can type in values in the Min and Max fields directly.

Clip Surface

contains a list of surfaces from which you can select the surface to be clipped.You must select a surface

to make the Clip button available.

designates the name of the surface to be created.The default is the concatenation of the surface type

and an integer which is the new surface ID.

Clip

creates the clipped surface. (The original surface will remain unchanged.)

Compute

computes the minimum and maximum values of the scalar field across the domain, and displays them

in the Min and Max boxes.

Manage...

opens the Surfaces Dialog Box (p. ) in which you can rename and delete surfaces and determine their

sizes.

The Iso-Surface dialog box allows you to interactively create isosurfaces. These surfaces can be isovalued

sections of an existing surface or of the entire domain. For more effective use of the slider bar, press

the Compute button before using it. See Isosurfaces (p. ) for details about the items below.

Controls

Surface of Constant

contains a list from which you can select the scalar field which will be used for isosurfacing.

Min

displays the minimum field value, which is computed when you click Compute.

Max

displays the maximum field value, which is computed when you click Compute.

Iso-Values

sets user-specified isovalues.There are two ways you can set the Iso-Values:

You can set an isovalue interactively by moving the slider with the left mouse button.This will also

create a temporary isosurface in the graphics window. Using the slider allows you to preview the

isosurfaces before defining them. Note: Even though the isosurface is displayed, it is only a temporary

surface.To create an isosurface, use the Create button after deciding on a particular isovalue.

Multiple isovalues will be contained in a single isosurface; that is, you cannot select subsurfaces within

the resulting isosurface.

From Surface

contains a list of existing surfaces from which you can select the surface to be used for isosurfacing. If

you do not select a surface from the list, the isosurfacing will be performed on the entire domain.

From Zones

contains a list of cell zones from which you can select the zone for creating an isosurface.

designates the name of the surface to be created.The default is the concatenation of the scalar field name

Create

creates the surface.

Compute

computes the minimum and maximum of the scalar field across the domain and displays them in the

Min and Max boxes.

Manage...

sizes.

The Iso-Value Adaption dialog box allows you to mark or refine cells inside or outside a specified

range of a selected scalar function. This dialog box is only available if you have used the following

text command: mesh/adapt/revert-to-R19.-user-interface; note that if you revert the

user interface, you cannot undo it in the current session, and some functionality is no longer available.

Domain → Adapt → Mark/Adapt Cells → Iso-Value...

Controls

Options

Controls

Options

contains radio buttons that control whether the cells inside or outside the isovalue range are marked for

Inside

enables the marking of cells with values between Iso-Min and Iso-Max.

Outside

enables the marking of cells with values less than Iso-Min or greater than Iso-Max.

Iso-Values of

contains a list from which you can select the solution variable to be used in the isovalue adaption function.

Min/Max

displays the minimum and maximum cell values of the selected field variable.The real number field values

Iso-Min

defines the minimum isovalue threshold.

Iso-Max

defines the maximum isovalue threshold.

Manage...

Adapt

adapts the mesh based on the isovalues of the selected solution variable, the isovalue ranges, and the

Inside/Outside option.

Mark

marks cells to be refined based on the isovalues of the selected quantity, the isovalue ranges, and the

Inside/Outside option.This command produces an adaption register.

Compute

computes the minimum and maximum cell values of the selected solution variable and displays them in

the Min and Max real number fields.

Solution → Reports → Definitions → New → Force Report → Lift...

Controls

Options

Per Zone

Controls

Options

Per Zone

specifies whether or not the lift for multiple walls zones should be monitored on each wall zone

separately.When this option is turned off (the default), Fluent computes and monitors the total lift

(optional) To have Fluent calculate a running average for the Lift Report Definition you can enter a

X,Y,Z

Create

Frequency

Frequency

op.

Lift Force

Wall Zones

lists the zones you can select for lift coefficient or drag lift computation.

OK

Compute

The Line/Rake Surface dialog box allows you to interactively create line and rake surfaces. A rake is

a linear, uniform distribution of points between two endpoints. See Line and Rake Surfaces (p. ) for

Controls

Options

contains options related to the line tool. See Using the Line Tool (p. ) for details about using this feature.

Line Tool

enables the line tool.

Reset

resets the line tool to its default position.

Type

selects line or rake as the surface to be created.

defines the number of points in the rake surface (inactive for line surfaces).

End Points

designates the coordinates of the first point (x0, y0, z0) and the last point (x1, y1, z1).

Select Points with Mouse

allows you to select endpoints with the mouse.You can select endpoints by clicking on locations in the

active window with the mouse-probe button. (See Controlling the Mouse Button Functions (p. ) for

information about setting mouse button functions.)

designates the name of the new surface.The default is the concatenation of the surface type and an integer

which is the new surface ID.

Create

Manage...

sizes.

The Manage Adaption Registers dialog box provides an interactive mechanism for creating, destroying,

and displaying functions for mesh adaption. This dialog box is only available if you have used the fol-

lowing text command: mesh/adapt/revert-to-R19.-user-interface; note that if you revert

the user interface, you cannot undo it in the current session, and some functionality is no longer

Domain → Adapt → Manage Registers...

Controls

Register Actions

contains operations applied to adaption or mask registers.

Change Type

toggles the register between adaption and mask types. Adaption registers are used to initiate refining

or coarsening of the mesh.Typically, mask registers are combined with adaption registers to control

the scope of the adaption process.

Combine

combines the selected adaption registers to create a hybrid adaption function. In some instances,

three new registers may be created: a combination of the adaption registers, a combination of the

mask registers, and then a combination of the two combined registers.

Delete

permanently discards the selected registers.

Mark Actions

Delete

contains operations applied to the cell markings defined in an adaption or mask register.

Exchange

modifies the cell markings in the following manner: all cells originally marked for refinement are

marked for coarsening, and all cells originally marked for coarsening are marked for refinement.

Invert

modifies all the cell markings in a mask register in the following manner: all cells that were originally

marked as ACTIVE are marked INACTIVE, and all cells originally marked as INACTIVE are marked ACTIVE.

Note that this action can only be applied to mask registers.

Limit

applies the adaption volume limits to the selected registers.

Fill

marks for coarsening all cells in the adaption register that are not marked for refinement.

Registers

contains a list from which you can select the current adaption and mask registers.The availability of many

of the actions in the dialog box is based on the number and/or type of adaption registers selected.

Register Info

provides the name, ID, number of cells marked for refinement and coarsening, and the type of the most

recently selected or deselected register.

opens the Adaption Display Options Dialog Box (p. ).

Adapt

adapts the mesh based on the selected adaption register.The Adapt button is not available if more than

one adaption register is selected. Adaption functions composed of combinations of adaption registers

can be produced using commands in the Register Actions and Mark Actions boxes.

Display

displays the cells marked for adaption in the selected adaption register in the active graphics window.

The Display button is not available if more than one adaption register is selected. Adaption functions

composed of combinations of adaption registers can be produced using commands in the Register Actions

and Mark Actions boxes.

The Merge Zones dialog box allows you to merge multiple zones of the same type into a single zone.

See Merging Zones (p. ) for details.

Controls

Multiple Types

contains a selectable list of the zone types for which you can merge multiple zones.You select a type

and the corresponding zones of that type will be displayed in the Zones of Type list.

Zones of Type

contains a list from which you can select two or more zones to be merged into a single zone.The zones

are of the type selected in the Multiple Types list.

Merge

merges the selected zones into a single zone. If your case file has dynamic zones or mesh interfaces, the

Warning Dialog Box (p. ) will open and require your input prior to the merge.

The Mesh Adaption Controls dialog box allows you to set limits on the minimum cell size, the min-

imum and maximum number of cells, and the cell types that can be adapted. In addition, it allows you

to vary the volume weighting of the gradient adaption function. This dialog box is only available if

you have used the following text command: mesh/adapt/revert-to-R19.-user-interface;

note that if you revert the user interface, you cannot undo it in the current session, and some function-

ality is no longer available.

Domain → Adapt → More → Controls...

Controls

Options

contains check buttons that control the manner in which the mesh can be adapted.

Refine

toggles mesh adaption by adding points.

Coarsen

toggles mesh adaption by removing points.

Zones

contains a list of cell zones from which you can select the zones in which to perform adaption (or marking).

By default, all cell zones are selected.

Min Cell Volume

Min # of Cells

specifies the minimum number of cells required in the mesh.

Note

When using the parallel solver, the Min # of Cells value is not strictly obeyed, but

provides an approximate limit to the minimum cell count that the adaption algorithm

will allow.

Max # of Cells

limits the total number of cells allowed in the mesh. A value of zero places no limits on the number of

cells.

Note

When using the parallel solver, the Max # of Cells value is not strictly obeyed, but

provides an approximate limit to the maximum cell count that the adaption algorithm

Max Level of Refine

specifies the maximum level of refinement for the cells.

Volume Weight

controls the volume weighting in the gradient adaption function.Valid values are between  and :  for

no volume weighting and  for full volume weighting.

The Mesh Interfaces dialog box allows you to automatically or manually create mesh interfaces for

use with sliding meshes (see Using Sliding Meshes (p. )) or multiple reference frames (see Mesh

Setup for a Multiple Moving Reference Frame (p. )), or for meshes with non-conformal boundaries

(see Non-Conformal Meshes (p. )). For information about using this dialog box, see Using a Non-

Conformal Mesh in ANSYS Fluent (p. ).

Domain → Interfaces → Mesh...

Controls

Unassigned Interface Zones

allows you to create new mesh interfaces using the automatic or manual method. Note that the selection

list at the top of the group box (which lists interface zones that have not yet been assigned to an existing

mesh interface) is only used as part of the automatic method.

Interface Name Prefix

specifies the prefix used in the names of all the mesh interfaces created automatically through the

Auto Create button.

opens the Auto Create Options Dialog Box (p. ), so you can define settings that you want applied

to the mesh interfaces that are created automatically through the Auto Create button.

Auto Create

creates mesh interfaces using the automatic method, so that Fluent is responsible for determining

which of the selected Unassigned Interface Zones can be grouped together to form the two sides

of one or more mesh interfaces. Note that mesh interfaces that use the periodic or periodic repeat

option cannot be created using this button, but must instead be created through the Manual Create...

button.

Manual Create...

opens the Create/Edit Mesh Interfaces Dialog Box (p. ), so you can create mesh interfaces using

the manual method. Note that this method is only necessary for mesh interfaces that use the periodic

or periodic repeat option.

allows you to manage existing mesh interfaces. Note that many of the buttons in this group box are not

accessible unless you make a selection from the list at the top.

Edit...

opens the Edit Mesh Interfaces Dialog Box (p. ), so you can edit the name, the list of interface zones

assigned to the interface, and/or the interface options.

List

prints information about the selected mesh interface in the console.When you click this button, ANSYS

Fluent will list the two interface boundaries and (if you have initialized the solution) all new zones

Delete

deletes the selected mesh interface. Note that this button can only be used on one mesh interface

at a time; if you would instead like to delete multiple interfaces in a single action, you can select them

in the tree and use the right-click menu command.

Draw

allows you to display the selected mesh interface (along with any additional selections in the Unas-

signed Interface Zones and/or Interface Zones lists) in the graphics window.

opens the Mesh Motion Dialog Box (p. ).

opens the Interface Options Dialog Box (p. ), where you can update which mesh interfaces use the

mapped option and set global parameters for the mapped mesh interfaces.

highlights the interface zones assigned to the mesh interface selected in the Mesh Interfaces group box,

and allows you to select specific interface zones to be displayed in the graphics window using the Draw

button.

The Mesh Morpher/Optimizer dialog box allows you to use the mesh morpher/optimizer to deform

the mesh in order to solve shape optimization problems. You can deform the mesh manually, allow a

built-in optimizer to define the deformation in order to minimize an objective function, or use Design

Exploration in ANSYS Workbench to easily explore a variety of deformation scenarios. See Using the

Mesh Morpher/Optimizer (p. ) for further details.

Design → Parameter-Based → Optimizer...

Controls

Regions

tab allows you to define the regions of the domain where the mesh will be deformed in order to optimize

the shape.

Control Point Distribution

allows you to select the way in which you will define the locations of the control points, as well as

the kinds of motions you can apply.

Regular

specifies that the control points will be spread in a regular distribution throughout the entire

deformation region.The number of control points along each of the defining direction vectors

will be specified in the Control Points group box.The motion of the control points will be limited

to translations, as the ability to define rotational or radial motions will not be available.

specifies that control point locations will be specified by right-clicking with the mouse on

boundary zones, distributing an approximate number throughout a zone, or by entering

coordinates, using the Define Control Points Dialog Box (p. ). The motion of the control

points will be able to be defined as translations, as rotations about a point / axis, or radially

about a point / axis.

Name

provides controls for the deformation regions you are defining.The upper text-entry box defines the

name of the region that is created when you click the Create button.The lower selection list allows

you to select a region that has already been created, in order to display it in the graphics window,

modify the settings via the Modify button, or delete the region via the Delete button.

Update from Zones

allows you to create a bounding box that defines the deformation region.

specifies the boundary zones that will be used to generate a bounding box for the deformation

region when you click the Define button.

Define

updates the values in the Origin, Direction- Vector, Direction- Vector, and Size of Region

group boxes based on a bounding box that encompasses the selections in the Boundary Zones

list, and previews the bounding box in green in the graphics window.

Enlarge

increases the size of the bounding box created by the Define button, and previews the revised

bounding box in green in the graphics window.

Reduce

Enlarge

Reduce

decreases the size of the bounding box created by the Define button, and previews the revised

updates the values in the Direction- Vector and Direction- Vector group boxes based on the

settings in the plane tool. See Using the Plane Tool (p. ) for information about the plane tool.This

button is only available for 3D cases.

Update from Line Tool

settings in the line tool. See Using the Line Tool (p. ) for information about the line tool.This button

is only available for 2D cases.

Origin

allows you to define the Cartesian coordinates of the origin of the deformation region.

X

defines the x coordinate of the origin of the deformation region.

Y

defines the y coordinate of the origin of the deformation region.

Z

defines the z coordinate of the origin of the deformation region.This number-entry box is only

available for 3D cases.

Direction- Vector

allows you to define a vector that acts as the first direction of the deformation region relative to the

Origin.

X

defines the x component of the first direction vector of the deformation region.

Y

defines the y component of the first direction vector of the deformation region.

Z

defines the z component of the first direction vector of the deformation region.This number-

entry box is only available for 3D cases.

defines a vector that is used to calculate the second direction of the deformation region relative to

the Origin. For 2D cases, the values in the Direction- Vector group box are automatically defined

by ANSYS Fluent to be perpendicular to the Direction- Vector. For 3D cases, the vector defined by

the Direction- Vector group box is projected onto a plane that intersects the Origin and is perpen-

dicular to the vector defined in the Direction- Vector group box, in order to calculate the second

X

defines the x component of the vector used to calculate the second direction of the deformation

region.This number-entry box is only editable for 3D cases.

Y

defines the y component of the vector used to calculate the second direction of the deformation

Z

defines the z component of the vector used to calculate the second direction of the deformation

region.This number-entry box is only available for 3D cases.

Size of Region

allows you to define the overall dimensions of the deformation region.

Direction-

defines the length of the deformation region along the direction specified by the Direction-

Vector group box.

defines the length of the deformation region along the third axis (that is, the cross product of the

vectors defined by the Direction- Vector and Direction- Vector group boxes).This number-

Boundary Continuity

allows you to specify whether the mesh transitions are smooth or abrupt wherever the mesh intersects

with the limits of the deformation region.This group box is only available when Unstructured is se-

lected from the Control Point Distribution list.

Smooth Transitions

enables smooth mesh transitions wherever the mesh intersects with the limits of the deformation

region, based on the creation of stationary control points at those intersections.

Display Control Points

displays the stationary control points created when the Smooth Transitions option is enabled.

allows you to define the control points for the deformation regions.

defines the number of control points for the deformation region selected in the Name group box

along the direction specified by the Direction- Vector group box.This number-entry box is only

available when Regular is selected from the Control Point Distribution list.

along the third axis (that is, the cross product of the vectors defined by the Direction- Vector

and Direction- Vector group boxes).This number-entry box is only available for 3D cases when

Regular is selected from the Control Point Distribution list.

Define...

Define...

opens the Define Control Points Dialog Box (p. ), which you can use to define the control points.

This button is only available when Unstructured is selected from the Control Point Distribution

list.

Preview

displays (in green) the bounding box that results from the current settings in the Origin, Direction-

Vector, Direction- Vector, and Size of Region group boxes.

Create

creates a new deformation region with the name specified in the upper text-entry box of the Name

group box and with the settings defined using the Origin, Direction- Vector, Direction- Vector,

Size of Region, and (for regular control point distributions) Control Points group boxes.The newly

created deformation region will be added to and selected in the lower Name selection list, and will

be displayed (in blue) in the graphics window.

Modify

modifies the saved settings for the deformation region selected in the lower Name selection list and

displays the modified region in the graphics window.

Delete

deletes the deformation region selected in the lower Name selection list.

tab allows you to define the constraints on the boundary zones, in order to limit the freedom of particular

zones that fall within the deformation region(s) during the morphing of the mesh.

Zones

allows you to select the boundary zones for which you are defining a constraint.

Option

specifies the constraint on the boundary zones selected from the Zones list.

Unconstrained

specifies that the boundary zones are completely free to be deformed according to the assigned

Passive

Passive

specifies that the nodes of the boundary zones are partially constrained to varying degrees, based

on their proximity to adjacent boundary zones that are fixed.The nodes in a passive boundary

zone behave in a similar manner to the interior mesh nodes, in order to ensure that there is a

smooth transition between fixed and unconstrained boundary zones.

Fixed

specifies that the boundary zones are fixed and will not be deformed.

Display

displays the selected Zones in the graphics window.

Summary

prints a list in the console that summarizes the constraint definitions for all of the boundary zones.

Deformation

tab allows you to define the deformation.

Number of Parameters

defines the number of parameters available to define the motion of the control points.

Parameter Values

allows you to define either the magnitude of deformation associated with each parameter (when you

are manually specifying the deformation or using Design Exploration in ANSYS Workbench to explore

multiple deformation scenarios) or the bounds for each parameter (when you are using a built-in

optimizer).

par1, par2...

specify the magnitude of deformation associated with each parameter.You can enter a numeric

value in the field or use the

icon to create or assign an input parameter (see Select Input Para-

meter Dialog Box (p. ) for details).These fields and icons are only available when none or

workbench is selected from the Optimizer drop-down list in the Optimizer tab. Note that the

value entered here will specify a length in meters for translations and radial motions, and will

specify an angle in degrees for rotations; these units will be used regardless of what units you are

using in the case.

Apply

saves definitions for the parameter fields in the Parameter Values group box.This button is only

available when none or workbench is selected from the Optimizer drop-down list in the Optim-

izer tab.

Set Bounds...

opens the Parameter Bounds Dialog Box (p. ), where you can define strict minimum and max-

imum values for the parameters. Note that this button is not available when workbench is selected

from the Optimizer drop-down list in the Optimizer tab.

Motion Settings...

opens the Motion Settings Dialog Box (p. ), where you can define the motion of the control points.

Deform

applies the current settings in the Parameter Values group box, modifies the mesh, and updates the

mesh display in the graphics window.This button is only available when none is selected from the

Optimizer drop-down list in the Optimizer tab.

Check

displays a mesh check report in the console for the mesh displayed in the graphics window.This

button is only available when none is selected from the Optimizer drop-down list in the Optimizer

tab.The mesh check report provides volume statistics, mesh topology and periodic boundary inform-

ation, verification of simplex counters, and verification of node position with reference to the  axis

for axisymmetric cases, in the same manner as the Check button in the General task page (see

Checking the Mesh (p. ) for details).

Reset

Reset

undoes any modifications made to the mesh as a result of the Deform button and updates the mesh

display in the graphics window.

Optimizer

tab allows you to define the settings for the optimizer.

Optimizer

specifies which optimizer is used.The choices include none (for manual deformation); compass,

newuoa, powell, rosenbrock, simplex, and torczon (for optimization in ANSYS Fluent); and work-

bench (for optimizing using Design Exploration in ANSYS Workbench). Note that workbench is only

available if you have launched your ANSYS Fluent session from ANSYS Workbench. For information

about how the built-in optimizers function or how to use Design Exploration, see Design Analysis

and Optimization (p. ) in the User's Guide or Working With Input and Output Parameters in Work-

bench in the ANSYS Fluent in Workbench User's Guide, respectively.

Objective Function Definition...

opens the Objective Function Definition Dialog Box (p. ), where you can specify the format of the

objective function that will be minimized during the optimization process.This button is not available

if none or workbench is selected from the Optimizer drop-down list.

Optimizer Settings

allows you to specify the optimizer settings.This group box is not available if none or workbench is

selected from the Optimizer drop-down list.

Maximum Number of Designs

defines the maximum number of design stages the optimizer will undergo to reach the specified

objective function.

Maximum Iterations per Design

defines the maximum number of iterations ANSYS Fluent will perform for each design change.

Optimizer Convergence Criteria

defines the convergence criteria for the optimizer.

Initial Parameter Variation

defines how much the parameters will be allowed to vary during the initial calculations when

newuoa is selected from the Optimizer drop-down list.

Mesh Quality

allows you to enable and define a mesh quality check: if the orthogonal quality (as defined in Mesh

Quality (p. )) for any cell of a mesh is less than a specified value, no solution is calculated for the

mesh and Fluent proceeds to the next design stage.This group box is not available if none is selected

from the Optimizer drop-down list.

Reject Poor Quality Meshes

enables the consideration of orthogonal quality when determining whether a solution should be

calculated for a mesh.

defines the minimum orthogonal quality value every cell must have in order for a solution to be

calculated for a mesh.Values may range from – (where  represents the worst quality).

Case and Data File Sets

allows you to enable the automatic saving of intermediate case and data files at specified intervals

during the optimization run, so that you can restart an interrupted solution in the same or a different

Fluent session without increasing the overall number of design iterations needed to reach convergence.

This group box is not available if none or workbench is selected from the Optimizer drop-down list.

Save Every

specifies the frequency (in number of design iterations) that you want intermediate case and data

file sets saved. Note that the default value is , which specifies that no intermediate files will be

saved.

Maximum Number Retained

specifies the maximum number of intermediate case and data files sets you want to retain. After

the maximum limit of file sets has been saved, ANSYS Fluent begins overwriting the earliest existing

intermediate file set.

File Name

specifies a root name for the intermediate case and data file sets, which will be appended with a

number that represents the design iteration during which it was saved. Note that you can include

a folder path in the file name if you want the files saved outside of the working folder.

provides settings that determine how the solution variables are treated after the mesh is deformed

during the optimization process.This group box is not available if none or workbench is selected

Method

allows you to select one of the following:

Initialize Data After Morphing

specifies that the solution variables should be initialized to the values defined in the Solution

Initialization task page after deformation.

Continue with Current Data

specifies that the solution variables should remain the values obtained in the previous design

Read Data File After Morphing

specifies that the solution variables are set to the values obtained from the data file specified

in the Data File Name text-entry box after deformation.This selection is not available when

Data File Name

specifies the data file from which the solution variables are obtained when Read Data File After

Morphing is selected.

allows you to specify commands (text commands or command macros) that will be run during the

optimization runs of the mesh morpher/optimizer.This group box is not available if none, newuoa,

or workbench is selected from the Optimizer drop-down list.

Initial Commands

specifies the commands that will be run after the design has been modified, but before ANSYS

Fluent has started to run the calculation for that design stage.

End Commands

specifies the commands that will be run after the solution has run and converged for a design

stage.

Monitor...

opens the Optimization History Monitor Dialog Box (p. ), which allows you to plot and/or record

how the value of the objective function varies with each design stage.This button is not available if

none, newuoa, or workbench is selected from the Optimizer drop-down list.

Apply

saves the settings in the Optimizer tab.

Summary

displays a summary of the mesh morpher/optimizer settings in the console.

Optimize

initiates the optimization process using the settings saved in all of the tabs of the Mesh Morpher/Op-

timizer dialog box.This button is not available if none or workbench is selected from the Optimizer

The Mixing Planes dialog box allows you to define the mixing planes for a mixing plane model. See

Setting Up the Mixing Plane Model (p. ) for details about using the items below.

Controls

Mixing Plane

contains a list from which you can select an existing mixing plane, and an informational field in which

Controls

ANSYS Fluent displays the name of the currently selected (or most recently created) mixing plane.

Upstream Zone, Downstream Zone

contain lists from which you can select the boundaries on the upstream and downstream sides of the

mixing plane, and informational fields that show the names of the zone you selected in each list. (You

cannot edit these fields; the name in each field will be the name of the zone you selected in the list below

it.)

Interpolation Points

specifies the number of radial or axial locations used in constructing the boundary profiles for circumfer-

ential averaging.This item appears only in 3D.

Mixing Plane Geometry

defines the geometry of the mixing plane interface.This item appears only in 3D.

Radial

specifies that information at the mixing plane interface is to be circumferentially averaged into profiles

that vary in the radial direction, for example,

,

.

Axial

specifies that circumferentially averaged profiles are to be constructed that vary in the axial direction,

for example,

,

.

Global Parameters

contains parameters related to the mixing plane calculation.

Averaging Method

consists of three profile averaging methods.

Area

is the default method and is expressed using Equation . in the Theory Guide.

Mass

provides better representation of the total quantities than the area averaging method. It is defined

by Equation . of the Theory Guide.

Mixed-Out

is most representative of non-uniform flow profiles and is expressed using Equation . in the

Under-Relaxation

Mixed-Out

specifies the under-relaxation factor for updating the boundary values at mixing planes.

Apply

sets the specified Under-Relaxation.

Default

sets the Under-Relaxation to its default value, as assigned by ANSYS Fluent. After execution, the

Default button becomes the Reset button.

Reset

resets the Under-Relaxation to its most recently saved value (that is, the value before Default was

selected). After execution, the Reset button becomes the Default button.

Create

creates the specified mixing plane (and assigns it a name in the Mixing Plane field).

Delete

deletes the mixing plane selected under Mixing Plane.

Solution → Reports → Definitions → New → Force Report → Moment...

Controls

Options

Per Zone

specifies whether or not moments for multiple walls should be monitored on each wall separately.When

this option is turned off (the default), Fluent computes and monitors the total force for all of the se-

lected walls combined together.

(optional) To have Fluent calculate a running average for the Moment Report Definition you can

contains the Cartesian coordinates of the moment center.

contains the Cartesian coordinates of the moment vector to be monitored.

Create

Frequency

op.

Moment Coefficient

Moment

Wall Zones

lists the zones you can select for moment computation.

Highlight Zones

when enabled, highlights the selected Wall Zones in the graphics window.

OK

Compute

OK

Compute

The Motion Settings dialog box allows you to define the motion of the control points, as part of the

definition of the deformation produced by the mesh morpher/optimizer. Note that the controls and

workflow of this dialog box are very much dependent on the selection in the Control Point Distribution

list in the Regions tab of the Mesh Morpher/Optimizer dialog box. See Using the Mesh Morpher/Op-

timizer (p. ) for details about using this dialog box.

The Motion Settings dialog box is opened from the Mesh Morpher/Optimizer Dialog Box (p. ).

Controls (when Regular is selected from the Control Point Distribution list in the Regions tab of

the Mesh Morpher/Optimizer dialog box)

Region

selects the deformation region for which you are assigning parameters and translation directions to

control points.

defines the control points to which you are assigning parameters and translation directions.

Selection Tools

provides tools for selecting the control points to which you are assigning parameters and translation

allows you to specify the Control Points by clicking in the graphics window with the mouse-probe

button (which is the right mouse button, by default).

Indexed Grouping

allows you to select the control points based on their assigned indices.

i

allows you to select from a list of control point index numbers, which identify the location in a

sequence (starting at the origin of the region) of control points along the direction- vector (as

defined in the Regions tab of the Mesh Morpher/Optimizer dialog box).

j

k

defined—though not displayed—in the Regions tab of the Mesh Morpher/Optimizer dialog

box).

Select

adds the control points that satisfy the selected index criteria (that is, the selections from the i, j,

and k drop-down lists) to the list of selected Control Points.

Deselect

removes the control points that satisfy the selected index criteria (that is, the selections from the

i, j, and k drop-down lists) from the list of selected Control Points.

specifies the names of the parameters (whose values are displayed in the Parameter Values group box

in the Deformation tab of the Mesh Morpher/Optimizer dialog box) that you are assigning to the

Control Points.The products of the values associated with these parameters and the settings specified

in the Translation Direction group box define the displacement of the control points during manual

deformation.

Translation Direction

allows you to define coefficients in the x, y, and (for 3D cases) z directions to scale the magnitude of de-

formation for the selected parameters. If you use a built-in optimizer, these coefficients provide the dir-

ection of the displacement of the control points and the optimizer determines the overall magnitude of

displacement. Alternatively, if you manually specify the deformation or use Design Exploration in ANSYS

Workbench to explore multiple deformation scenarios, the values you enter in the Translation Direction

group box are multiplied with the values of the Parameters (as displayed in the Parameter Values group

box in the Deformation tab of the Mesh Morpher/Optimizer dialog box) to define the displacement of

the control points.

X

defines the scaling coefficient applied to the deformation parameter in the x direction.

Y

defines the scaling coefficient applied to the deformation parameter in the y direction.

Z

defines the scaling coefficient applied to the deformation parameter in the z direction.This number-

Apply

saves the selections made in the Parameters selection list and the values entered in the Translation

Direction group box, and assigns these parameter settings to the control points selected in the Control

Read...

allows you to define your motion settings by reading an ASCII text file. See Mesh Morpher/Optimizer File

Formats (p. ) for further details about the text file format.

Summary

displays a summary of the saved motion settings in the console.

Write...

allows you to write your saved motion settings to an ASCII text file. See Mesh Morpher/Optimizer File

Summary

Write...

Controls (when Unstructured is selected from the Control Point Distribution list in the Regions tab

of the Mesh Morpher/Optimizer dialog box)

Name

provides controls for the motions you are defining.The upper text-entry box defines the name of the

motion that is created when you click the Create button (which by default is based on the type of motion

and the related parameter).The lower selection list allows you to select a motion that has already been

created, in order to display the selections associated with it, or to modify or delete the motion using the

Modify or Delete buttons, respectively.

Parameter

allows you to select the parameter (whose value is displayed in the Parameter Values group box in the

Deformation tab of the Mesh Morpher/Optimizer dialog box) for the motion.

Type

allows you to specify the type of motion you want to define.

specifies that the motion is a translation, based on the settings in the Direction group box.

Rotation

specifies that the motion is a rotation about a point (for 2D) or an axis (for 3D), based on the settings

in the Axis Origin group box and (for 3D cases) Axis Direction group box.

Radial

specifies that the motion is defined radially about a point (for 2D) or an axis (for 3D), based on the

settings in the Axis Origin group box and (for 3D cases) Axis Direction group box.

Direction

allows you to define coefficients in the X, Y, and (for 3D cases) Z directions to scale the magnitude of

Direction

deformation for the selected parameter. If you use a built-in optimizer, these coefficients provide the

direction of the displacement of the control points and the optimizer determines the overall magnitude

of displacement. Alternatively, if you manually specify the deformation or use Design Exploration in ANSYS

Workbench to explore multiple deformation scenarios, the values you enter in the Direction group box

are multiplied with the values of the Parameter (as displayed in the Parameter Values group box in the

Deformation tab of the Mesh Morpher/Optimizer dialog box) to define the displacement of the control

points.

This group box is only available when Translation is selected from the Type list.

allows you to define the X, Y, and Z components of the vector about which the control points will rotate

or move radially, when the selection in the Type list is Rotation or Radial, respectively.This group box

is only available for 3D cases.

allows you to define the X, Y, and (for 3D cases) Z coordinates of the origin about which the control points

will rotate or move radially, when the selection in the Type list is Rotation or Radial, respectively.

allows you to select the control points that will undergo the motion.

provides tools for selecting the control points that will undergo the motion.

Create

creates a new motion based on the currently displayed settings.

Modify

Create

Modify

modifies the saved settings for the motion selected in the lower Name selection list.

Delete

deletes the motion selected in the lower Name selection list.

Read...

allows you to define your motion definitions by reading an ASCII text file. See Mesh Morpher/Optimizer

File Formats (p. ) for further details about the text file format.

Summary

displays a summary of the saved motion definitions in the console.

Write...

allows you to write your saved motion definitions to an ASCII text file. See Mesh Morpher/Optimizer File

Setup → Boundary Conditions → <selected boundaries>

Multi-Edit...

Controls

Master Zone Name

non-editable field displaying the name of the "master" boundary, which cannot be deselected in the Zone

List. When the dialog box is first opened, the values of the "master zone" are shown in all fields.

Zone List

lists all of the zones that are compatible for multi-editing with the "master" zone.The selected zones are

the ones that will be modified on Apply.

indicates that the value of this setting varies between the selected boundaries in the Zone List.

indicates that the displayed value will be applied to the selected boundaries in the Zone List when you

click Apply.

Apply

applies the settings marked with the

icon to the selected boundaries in the Zone List.

Refer to Editing Multiple Boundary Conditions at Once (p. ) for additional information about this

functionality. Note that while this image shows the Multi Edit Velocity Inlet Settings dialog box, the

functionality that is specific to multi-editing is consistent across the different multi-edit dialog boxes.

For information on specific settings of boundary conditions, refer to Boundary Conditions Task

Page (p. ) (which contains descriptions of each boundary's dialog box), and Boundary Condi-

Click New... in the Report File Definitions dialog box to open the New Report File dialog box.

Controls

Name

Active

Add>>

<<Remove

File Name

Browse...

frequency for writing the file in units of time.Time-step and flow-time are only a valid choices when you

New

defined).

Edit...

Click New... in the Report Plot Definitions dialog box to open the New Report Plot dialog box.

Controls

Name

Active

Add>>

<<Remove

Options

Curves...

Axes...

Plot Title

New

defined).

Edit...

The Objective Function Definition dialog box allows you to specify the format of the objective

function that will be minimized by the mesh morpher/optimizer and (when it is a customized function

of output parameters) to define the objective function. See Using the Mesh Morpher/Optimizer (p. )

The Objective Function Definition dialog box is opened from the Mesh Morpher/Optimizer Dialog

Box (p. ).

Controls

Options

contains options for the format of the objective function.

specifies that the objective function is provided via a user-defined function.

Controls

Options

Scheme Procedure

specifies that the objective function is provided via a Scheme source file.This option is not available

if newuoa is selected from the Optimizer drop-down list in the Optimizer tab of the Mesh Morph-

er/Optimizer dialog box.

Custom Calculator

specifies that the objective function is based on output parameters, and is defined by the controls in

the Custom Calculator group box.This option is not available if newuoa is selected from the Optim-

izer drop-down list in the Optimizer tab of the Mesh Morpher/Optimizer dialog box.

allows you to define the objective function.This group box is only available when Custom Calculator is

selected from the Options list.

Function to Minimize

displays the objective function defined by the controls in the Custom Calculator group box.

Select Operand from

allows you to include output parameters in the definition of the objective function.

provides a list of available output parameters, which can be included in the definition of the ob-

jective function.

opens the Parameters Dialog Box (p. ), which you can use to create additional output parameters.

Refresh

updates the Output Parameters list, so that all available output parameters are displayed.

Select

enters the output parameter that is currently selected in the Output Parameters list in the

Function to Minimize field.

Operators

allows you to include calculator operators in the definition of the objective function. Clicking a button

Operators

in this group box causes the appropriate symbol to appear in the Function to Minimize field.

Apply

saves the custom objective function (displayed in the Function to Minimize field) as part of the case

file.

Clear

deletes all of the text in the Function to Minimize field.

The Optimization History Monitor dialog box allows you to plot and/or record optimization history

data, that is, how the value of the objective function (defined using the Mesh Morpher/Optimizer

Dialog Box (p. )) varies with each design stage produced by the mesh morpher/optimizer. See Using

the Mesh Morpher/Optimizer (p. ) for details about using this dialog box.

The Optimization History Monitor dialog box is opened from the Mesh Morpher/Optimizer Dialog

Box (p. ).

Controls

Plot

enables the plotting of the optimization history data in the graphics window (with the ID specified in

Window).

Window

sets the ID of the graphics window in which the plot will be displayed.This number-entry box is only

available when the Plot option is enabled.While ANSYS Fluent is iterating, the active graphics window

is temporarily set to this ID to update the optimization history plot, and then it is returned to its previous

value.Thus, the optimization history plot can be maintained in a separate window that does not interfere

with other graphical postprocessing.

Write

enables the saving of the optimization history data to a file (with the name specified in File Name).

File Name

Write

File Name

specifies the name of the file to which the optimization history data is written.This text-entry box is only

available when the Write option is enabled.

Plot

displays an XY plot of the optimization history data generated during the last calculation. Note that no

plot will be displayed if the data was discarded using the Clear button.

Clear

discards the optimization history data, including the associated files. Each of these actions must be con-

firmed in a Question Dialog Box (p. ).

The Parallel Connectivity dialog box prints the connectivity of the selected compute node. See

Checking Network Connectivity (p. ) for details.

Controls

Compute Node

indicates the compute node ID for which connectivity information is desired.

Print

prints information (in the console window) about the network connectivity for the selected compute

node.

The Parameter Bounds dialog box allows you to limit how much each parameter is allowed to deform

when using the mesh morpher/optimizer. See Using the Mesh Morpher/Optimizer (p. ) for details

about using this dialog box.

The Parameter Bounds dialog box is opened from the Mesh Morpher/Optimizer Dialog Box (p. ).

Controls

selects the parameters (created using the Deformation tab of the Mesh Morpher/Optimizer Dialog

Box (p. )) for which you are defining bounds.

Range

allows you to specify the bounds.

Unbounded

allows you to specify whether the selected Parameters are unbounded.

Range

Unbounded

Min, Max

allows you to set the minimum and maximum values allowed for the selected Parameters when the

Unbounded option is disabled.

Apply

saves the bounds for the currently selected Parameters.

Summary

displays a summary of all of the saved parameter bounds in the console.

The Particle Tracks dialog box controls the generation and display of discrete phase particles. See

Displaying of Trajectories (p. ) for details about the items below.

Results → Graphics → Particle Tracks → New...

Controls

Particle Tracks Name

is the name for a particle tracks definition.You can specify a name or use the default name  particle-

tracks-id.This control appears only for particle tracks definitions.

Options

contains the options described below:

specifies that node values should be interpolated to compute the scalar field at a particle location.

This option is turned on by default. See Choosing Node or Cell Values (p. ) for details.

Auto Range

specifies that the minimum and maximum values of the scalar field will be the limits of that field. If

this option is not selected, you can enter Min and Max values manually.These values determine the

range of the color scale.

Draw Mesh

XY Plot

enables the display of an XY plot along the particle trajectories for steady particle tracking and at the

XY Plot

current particle locations for unsteady tracking.When this option is selected, the Display push but-

ton will change to Plot.

(available only when XY Plot is on) activates the file-writing option.When this option is selected, the

Plot push button will change to Write.... Clicking on the Write... button will open The Select File

Dialog Box (p. ), in which you can specify a name and save a file containing the XY plot data.The

format of this file is described in XY Plot File Format (p. ).

Enable Filter

when activated allows you to click the Filter by....

Filter by...

opens the Particle Filter Attributes (p. ) where you can specify how you would like to filter the particles

being displayed.

Reporting

allows you to specify how you would like to report particle tracks.

controls the type of trajectory-fate reports to be displayed.

Off

disables reporting of trajectory fates.

Summary

enables summary reports of trajectory fates. See Reporting of Trajectory Fates (p. ) for details.

Step by Step

enables the step-by-step reporting of trajectories.This item will not appear if you have requested

unsteady tracking in the Discrete Phase Model Dialog Box (p. ). See Step-by-Step Reporting of

Trajectories (p. ) for details.

Current Positions

enables the reporting of the positions and velocities of all particles that are in the domain at the

current time.This item appears only when unsteady tracking has been requested in the Discrete

Phase Model Dialog Box (p. ). See Reporting of Current Positions for Unsteady Tracking (p. )

Report to

indicates the destination of the trajectory report.

File

enables the writing of the trajectory report to a file.When this option is enabled, the Track button

will become the Write... button.

Console

enables the display of the trajectory report information in the console window.

Significant Figures

controls the number of significant figures used when a Step by Step or Current Positions report is

selected.

Reporting Variables...

opens the Reporting Variables Dialog Box (p. ) that contains a list from which you can select the

scalar field to be used to color the particle tracks.

Track Style

sets the trajectory style.Trajectories can be displayed as lines, ribbons, spheres, cylinders, or a set of

points. Pulsing can be done only on point or line styles.

opens the Track Style Attributes Dialog Box (p. ), Particle Sphere Style Attributes Dialog Box (p. ),

or the Ribbon Attributes Dialog Box (p. ), depending on the selected Track Style.These dialog

boxes allow you to set the attributes for the chosen trajectory style.

Vector Style

sets the trajectory vector style.You can display the trajectories vectors in three different ways: vector,

centered-vector, and centered-cylinder. All three styles are demonstrated in Controlling the Vector

Style of Particle Tracks (p. ).

opens the Particle Vector Style Attributes Dialog Box (p. ).

Pulse Mode

Pulse Mode

specifies either a single or continuous release of particles that follow the trajectories, starting at the release

surface, when you use the Pulse button to animate the trajectories.

Continuous

sets the pulse mode to continuously release particles from the initial positions.

Single

sets the pulse mode to release a single wave of particles.

The Pulse Mode is used only when particles are being Pulsed.

contains a list of solution variables that can be used for the  axis of the plot.

This item appears when the XY Plot option is turned on.

contains a list of functions for the X-axis of the plot.You can plot the quantity selected in the Y Axis

Function drop-down list as a function of the Time elapsed along the trajectory, or the Path Length along

the trajectory.

Min/Max

display the values to which the lower and upper ends of the color scale map. If you are using the Auto

Range option, these values will be automatically computed when you click Compute. If you are not using

Auto Range, you can enter values manually.

Update Min/Max

computes the Min and Max for the field chosen in Color by.

Track PDF Transport Particles

enables the tracking of PDF transport particles.This item is available only when the composition PDF

transport model is enabled.

Free Stream Particles

enables the tracking of free stream particles. Note that this option is available only when the Lagrangian

wallfilm model is enabled in the wall boundary conditions dialog box, under the DPM tab.

Wall Film Particles

enables the tracking of wall film particles. Note that this option is available only when the Lagrangian

Track Single Particle Stream

enables the tracking of a single particle stream in the selected injection, instead of all the streams in that

injection. See Displaying of Trajectories (p. ) for details.

Stream ID

specifies the particle stream to be tracked when the Track Single Particle Stream option is enabled.

Skip

allows you to “thin” or “sample” the particles that are displayed.

Coarsen

reduces the plotting time by reducing the number of points that are plotted for a given trajectory in any

cell.This is valid only for steady-state cases.

Release from Injections

selects the injections from which to release particles.You must select at least one injection before any

particles can be released.

Display

displays the particle trajectories and generates a trajectory report in the console window (if requested)

for steady particle tracking. For unsteady particle tracking, only the current particle locations will be

shown.

displays the particle tracks (steady tracking) or the current particle locations (unsteady tracking) in the

active graphics window and saves the particle track definition.This button appears only for particle track

definitions and replaces the Display button.

Plot

displays an XY plot along the particle trajectories.This button replaces the Display button when the XY

Plot option is turned on.

Write...

Plot

Write...

opens The Select File Dialog Box (p. ), in which you can save the XY plot data or trajectory report to a

file.This button replaces the Plot button when the Write to File option is turned on, or the Track button

when the File option is selected under Report to.

Pulse

animates the position of particles. If Pulse Mode is set to Continuous, particles are reintroduced at the

seed positions repeatedly. If the mode is Single, a single wave of particles moves through the domain.

Pulse is not available for unsteady tracking.

The label of this button changes to Stop ! when the animation is in progress. Click Stop ! to stop

pulsing (and the label goes back to Pulse).

Track

computes the particle trajectories and generates any reports without displaying the trajectories in the

Axes...

opens the Axes Dialog Box (p. ), which allows you to customize the XY plot axes.This item appears

when the XY Plot option is turned on.

Curves...

opens the Curves Dialog Box (p. ), which allows you to customize the curves used in the XY plot.This

item appears when the XY Plot option is turned on.

The Partition Surface dialog box allows you to create a surface defined by the boundary of two adjacent

mesh partitions. See Partition Surfaces (p. ) for details about the items below.

Controls

Options

contains check buttons that allow you to choose interior or exterior faces or cells to be contained in the

partition surface.

Cells

Controls

Options

Cells

specifies, when enabled, that the partition surface will consist of cells (either interior or exterior, de-

pending on the status of the Interior check button) that lie on the partition boundary.When this

option is disabled, the faces on the boundary between partitions will make up the partition surface.

Depending on the status of the Interior check button, the faces will reflect data values for the interior

or exterior cells.

Interior

toggles between interior and exterior cells. If the partition surface consists of faces instead of cells,

Interior specifies for which cells data will be displayed on the faces.When this option is enabled, in-

terior cells (cells that are on the Int Part side of the partition boundary) will make up the partition

surface.When it is disabled, the partition surface will consist of exterior cells (cells that are on the Ext

Part side of the partition boundary).

contains information about which partitions are under consideration.The boundary that defines the

partition surface is the boundary between the Int Part and the Ext Part. If there are more than two mesh

partitions, each interior partition will share boundaries with several exterior partitions. By setting the ap-

propriate values for Int Part and Ext Part, you can create surfaces for any of these boundaries.

Min/Max

indicates the minimum and maximum ID numbers of the mesh partitions.The minimum is always

zero, and the maximum is one less than the number of processors.

Int Part

Min/Max

Int Part

indicates the ID number of the interior partition (that is, the partition under consideration).

Ext Part

indicates the ID number of the bordering partition.

Surfaces

displays an informational list of existing surfaces.

Create

Manage...

sizes.

The Partitioning and Load Balancing dialog box allows you to partition the mesh into separate

clusters of cells for separate processors on a parallel computer. See Partitioning the Mesh Manually

and Balancing the Load (p. ) for details.

The Partitioning and Load Balancing dialog box also allows you to enable and control ANSYS Fluent’s

load balancing feature. Load balancing will automatically detect and analyze parallel performance, and

redistribute cells between the existing compute nodes to optimize it. See Load Balancing (p. ) for

more information about load balancing.

Parallel → General → Partitioning/Load Balancing...

Controls

Method

Options

tab

Number of Partitions

defines the desired number of mesh partitions.This usually matches the number of processors available

for parallel computing.

Reporting Verbosity

specifies the amount of information to be reported in the text (console) window during the partitioning.

With the default value of , Fluent will print the number of partitions created, the number of bisections

performed, the time required for the partitioning, and the minimum and maximum cell, face, interface,

and face-ratio variations. (See Interpreting Partition Statistics (p. ) for details.) If you increase the

Reporting Verbosity to , the partition method used, the partition ID, number of cells, faces, and

interfaces, and the ratio of interfaces to faces for each partition will also be printed in the console

window. If you decrease the Reporting Verbosity to , only the number of partitions created and

the time required for the partitioning will be reported.

allows partitions to cross zone boundaries (the default). If turned off, it will restrict partitioning to

within each cell zone.This is recommended only when cells in different zones require significantly

different amounts of computation during the solution phase, for example if the domain contains both

solid and fluid zones.

Laplace Smoothing

enables the Laplace smoothing method, which can be used to prevent partition boundaries from lying

along regions of high-aspect ratio cells.This can improve convergence behavior in cases with highly

stretched cells.

Cutoff Aspect Ratio

controls the threshold for the Laplace smoothing method.

Reordering Method

is used to optimize parallel performance

Architecture Aware

is the default option and it accounts for the system architecture and network topology in

remapping the partitions to the processors.

Reverse Cuthill-McKee

minimizes the bandwidth of the compute-node connectivity matrix (the maximum distance

between two connected processes) without incorporating the system architecture.

Optimization

tab contains options for enabling schemes to optimize the partitions created by the selected partition

method. In addition, the optimization scheme will be applied until appropriate criteria are met, or the

maximum number of iterations have been run. If the Iterations counter is set to , the optimization

scheme will be applied until completion, without limit on the maximum number of iterations.

Merge

attempts to decrease the number of interfaces by eliminating orphan cell clusters (an orphan cluster

is a group of connected cells whose members each have at least one face coincident with an interface

boundary).

Smooth

attempts to minimize the number of interfaces by sacrificing cells on the partition boundary to the

neighboring partition to reduce the partition boundary surface area.

Smooth

Pre-Test

Weighting

tab allows you to set the appropriate weights, prior to partitioning the mesh.

Weight Types

allows you to turn on/off a specific weight. Weight types include: Faces per Cell (enabled by

default, with additional weighting of ), Solid Zones (available and enabled by default only if

solid cell zones are defined); VOF (available only if the volume of fluid multiphase model is

turned on); DPM (available only for discrete phase simulations with injections defined), where

you can specify Hybrid Optimization; and ISAT.

allows you to specify that ANSYS Fluent timers set the weight scaling (by not enabling the

check box), or to modify the value yourself (by enabling the check box and entering a numer-

ical value in the Value field.

Value

allows you to enter a user-specified numerical value to modify the weighting set by the ANSYS

Fluent timers. Note that for VOF, DPM, and ISAT, this value is not relevant when using model-

weighted partitioning.

Dynamic Load Balancing

tab allows you to set load balancing thresholds and intervals.

allows you to set thresholds and intervals for the simulation’s physical models.

Threshold

is a percentage and depending on the value, load balancing will occur if the load imbalance is

greater than the value entered.

Threshold

Interval

allows you to specify the desired interval for load balancing cycles, in terms of number of iterations.

When a value of  is specified, ANSYS Fluent will internally determine the best value to use, initially

using an interval of  iterations.You can override this behavior by specifying a nonzero value.

ANSYS Fluent will then attempt to perform load balancing after every N iterations, where N is the

specified Balance Interval.

allows you to set load balancing threshold and interval values for your dynamic mesh.This option is

only available when the dynamic mesh model is enabled.

Auto

allows a percentage of interface faces and loads to be automatically traced.

Threshold

Interval

Mesh Adaption

allows you to set threshold values for mesh adaption.

Threshold

Zones

contains a list of cell zones. Partitioning will be applied to cells in zones selected from this list.

Registers

Zones

Registers

contains a list of cell registers that have been created using the adaption tools.You can restrict partitioning

to a group of cells by selecting a register containing the cells. See Partitioning Within Zones or Re-

gisters (p. ) for details.

Print Active Partitions

prints the partition ID, number of cells, faces, and interfaces, and the ratio of interfaces to faces

for each active partition (see Checking the Partitions (p. ) for information about active partitions)

in the console. In addition, it prints the minimum and maximum cell, face, interface, and face-ratio

variations.

Print Stored Partitions

for each stored partition (see Checking the Partitions (p. ) for information about stored partitions)

Set Selected Zones and Registers to Partition ID

allows you to set a value that assigns selected Zones and/or Registers to a specific partition ID. A region

or zone is marked before setting the marked cells to one of the partition IDs.

Use Stored Partitions

allows you to make the stored cell partitions the active cell partitions in a parallel session. The

active cell partition is used for the current calculation, while the stored cell partition (the last par-

tition performed) is used when you save a case file.

Partition

subdivides the mesh into the selected number of partitions using the prescribed method and optimiza-

tion(s).

Default

Partition

tion(s).

Default

sets all controls to their default values, as assigned by ANSYS Fluent. After execution, the Default button

Reset

The Pathlines dialog box controls the generation and display of pathlines. See Displaying Path-

lines (p. ) for details about the items below.

Results → Graphics → Pathlines → New...

Controls

Pathline Name

is the name for a pathline definition.You can specify a name or use the default name  pathline-id.

This control appears only for pathline definitions.

Options

Oil Flow

toggles between regular pathlines and oil-flow pathlines.When this option is selected, pathlines are

constrained to lie on the zone selected in the On Zone list.

Reverse

specifies that each particle’s path is traced back in time.This option is turned off by default.

Auto Range

Draw Mesh

Draw Mesh

when enabled opens the Mesh Display Dialog Box (p. ) where you can specify how to display your

mesh.

allows you to specify tolerance to control the pathlines accuracy.

Relative Pathlines

allows you to display the pathlines relative to the rotating reference frame.

XY Plot

enables the display of an XY plot along the pathline trajectories.When this option is selected, the

Display push button will change to Plot.

activates the file-writing option.When this option is selected, the Type option becomes active and

the Plot push button will change to Write.... Clicking on the Write... button will open The Select File

Type

CFD-Post

allows you to write the file in CFD-Post compatible format, which can be read in CFD-Post.

Fieldview

Geometry

allows you to write the file in .ibl format, which can be read in GAMBIT.

EnSight

allows you to write the file in .encas format, which can be read in EnSight.

Pulse Mode

specifies either a single or continuous release of particles that follow the pathlines, starting at the release

surface, when you use the Pulse button to animate the pathlines.

Single

Single

The Pulse Mode is used only when particles are being pulsed.

Style

sets the pathline style. Pathlines can be displayed as lines, ribbons, spheres, cylinders, or a set of points.

The ribbon style also uses the Twist By field and the TwistFactor value (specified in the Ribbon Attributes

Dialog Box (p. )). Pulsing can be done only on point or line styles.

opens the Path Style Attributes Dialog Box (p. ) or the Ribbon Attributes Dialog Box (p. ), depending

on the selected Style.These dialog boxes allow you to set the attributes (ribbon width, marker size, cyl-

inder radius, twist-by field, and so on) for the chosen pathline style.

Step Size

sets the interval used for computing the next position of a particle.This is in units of length. Particle pos-

itions are always computed when they enter/leave a cell. If you specify a very large size, the particle pos-

itions at entry/exit of each cell will still be computed (and displayed).

Tolerance

allows you to control the error when using large time step sizes for the calculation.This is available when

Accuracy Control is selected under Options.

Steps

sets the maximum number of steps a particle can advance. A particle’s path may also end if it leaves the

domain.

Path Skip

allows you to “thin” or “sample” the pathlines that are displayed. See “Thinning” Pathlines (p. ) for details.

Path Coarsen

reduces the time and the number of points plotted in a pathline. Coarsening factor of ’n’ will result in

plotting of each ’n’th point for a given pathline in each cell.

On Zone

contains a list from which you can select the zone on which the particles are constrained to lie.This list

is activated only when the Oil Flow option is selected.

Track in Phase

(for the Eulerian Multiphase model only) allows you to select the phase or the mixture of all phases for

tracking particle pathlines.

Color by

contains a list from which you can select the scalar field to be used to color the pathlines.The default is

Particle ID, a unique ID for each particle.

contains a list of functions for the  axis of the plot.You can plot the quantity selected in the Y Axis

Min/Max

Release from Surfaces

selects the surfaces from which to release particles.You must select at least one surface before any particles

can be released.

when enabled highlights the surfaces (selected in the Pathlines dialog box) in the graphics window.

Point

Point

Line/Rake

Plane

Quadric

Iso-Clip

EnSight Encas File Name

allows you to specify a.encas file name if you selected EnSight under Type.

Browse...

opens The Select File Dialog Box (p. ) where you can select the .encas file.

Time Steps For EnSight Export

allows you to set the number of time levels that are available for animation in EnSight.

Display

displays the pathlines in the active graphics window.

plots the pathlines in the active graphics window and saves the pathline definition.This button appears

only for pathline definitions and replaces the Display button.

Plot

displays an XY plot along the pathline trajectories.This button replaces the Display button when the XY

Write...

opens The Select File Dialog Box (p. ), in which you can save the XY plot data to a file.This button re-

places the Plot button when the Write to File option is turned on.

Pulse

Compute

Axes...

Curves...

The Plane Surface dialog box allows you to interactively create a planar surface that cuts through the

domain. See Plane Surfaces (p. ) for details about the items below.

Controls

Options

contains options for defining the plane surface.

Aligned with Surface

enables the specification of a plane parallel to an existing surface.

Aligned with View Plane

enables the specification of a plane parallel to the current view in the active graphics window.

Point and Normal

enables the specification of a plane having a certain normal vector and passing through a specified

point.

Bounded

enables the creation of a bounded parallelepiped,  of whose  corners are the  points that define

the plane equation (or the  corners of the Plane Tool).

Sample Points

enables the specification of a point density along the  directions (of the parallelepiped).This creates

a uniformly distributed set of points on the plane. (This item is available only when the Bounded

option is enabled.)

Plane Tool

enables the plane tool. See Using the Plane Tool (p. ) for details.This option is not available if you

are using the Aligned With Surface or Aligned With View Plane option.

Plane Tool

Sample Density

specifies the density of points when the Sample Points option is enabled.

Edge , Edge

sets the point density along the two directions of the plane. (Edge  extends from point  to point ,

and edge  extends from point  to point .)

Select Points

allows you to select points with the mouse.You can select endpoints by clicking on locations in the active

window with the mouse-probe button. (See Controlling the Mouse Button Functions (p. ) for information

about setting mouse button functions.)

Reset Points

resets the plane tool to its default position.

Surfaces

contains a list of currently defined surfaces. If you choose the Aligned With Surface option, this will be-

come a selectable list, and you can choose the surface that you want the new plane surface to be aligned

with.

Points

contains boxes in which you can set the coordinates of the three points defining the planar surface.

x0, y0, z0

designates the coordinates of the first point.

x1, y1, z1

designates the coordinates of the second point.

x2, y2, z2

designates the coordinates of the third point.

Normal

contains boxes in which you can specify the components of the normal vector when the Point And

Normal option is enabled.

ix, iy, iz

designates the coordinates of the end point of the normal vector (the start point being , , ).

Create

Manage...

Create

Manage...

sizes.

The Point Surface dialog box allows you to interactively create point surfaces (surfaces containing a

single data point). See Point Surfaces (p. ) for details about the items below.

Controls

allows you to specify a local reference frame (if defined) for the point surface.

Options

contains options related to the point tool. See Using the Point Tool (p. ) for details about using this

feature.

Point Tool

enables the point tool.

Reset

resets the point tool to its default position.

designates the coordinates of the point in the surface (x0, y0, z0).

Select Point with Mouse

allows you to select the point with the mouse.You can select a point by clicking on a location in the

Create

Manage...

sizes.

The Quadric Surface dialog box allows you to interactively define quadric functions and create surfaces

sizes.

from them. Lines and circles are commonly used types of quadric functions, so additional support is

provided for defining them. See Quadric Surfaces (p. ) for details about using the items below.

Important

Note that your inputs for the quadric function must be in SI units.

Controls

Type

selects the type of quadric function. Presently, you may select Line/Plane, Circle/Sphere or a general

Quadric. Some of the control buttons take on different meanings for each of the three quadric function

types.

Line/Plane

specifies that the surface will consist of all points on the domain that satisfy the equation

, where

ix

is the coefficient of  in the quadric function.

iy

iz

distance

is the distance of the line/plane from the origin.

When you click the Update button in Quadric Function, the coefficients in the quadric

function will change to reflect your inputs.

Circle/Sphere

specifies that the surface will consist of all points in the domain that satisfy the equation

, where

x0,y0,z0

are the

coordinates of the center.

r

is the radius.

Quadric

specifies that the surface will consist of all points in the domain that satisfy the quadric function

, where  is the quadric function you define as shown below.You will enter value to the

right of the Type entry, but the coefficients in the quadric function are entered directly in the

Quadric Function box. Note that in 2D problems the z entries are ignored.

x2, y2, z2, xy, yz, zx, x, y, z

are the coefficients of the corresponding terms in the quadric function.

Quadric Function

contains the display of the quadric function and the Update button. If you select Line/Plane or

Circle/Sphere as the Type, the coefficients of the quadric function will be updated here when you click

the Update button.You will not be able to edit the values in the Quadric Function box directly. If you

select Quadric as the Type, you will enter the coefficients directly in this box, and the Update button

will be inactive.

Update

updates the coefficients in Quadric Function to reflect the current input.

Create

Manage...

sizes.

The Reduced Order Model dialog box allows you to enable the reduced order model (ROM) and select

which variables and zones to include in the ROM—refer to Creating Reduced Order Models

(ROMs) (p. ) additional information. You can also use it to evaluate a produced ROM as discussed

in Reduced Order Model (ROM) Evaluation in Fluent (p. ).

Controls

Setup tab

Variables

lists the variables that are available for creating the ROM.

Zones

Controls

Setup tab

Variables

Zones

lists all of the zones in your case.You can select from this list to tell the ROM where the selected variables

in the Variables list will be evaluated.

Add>>

adds the selected variables and zones to the ROM.

Selected for ROM

lists all of the selected variables and their associated locations for the ROM.

Delete

removes the selected variables and zones from the Selected for ROM list.

Evaluate tab

Parameters used for ROM creation:

lists all of the variables that were used in creation of the reduced order model (ROM).The Min-Max Range

on the right of the fields lists the accepted input ranges for the number entry fields.

Evaluate

evaluates the case using the values you specify for the listed parameters.

The Reference Frame dialog box allows you to create local reference frames either with the coordinates

and orientation that you specify or by tracking a cell zone. Refer to Reference Frames (p. ) additional

Controls

Definition Method

specifies how you want to define the reference frame.

Parent (User Defined only)

specifies the parent reference frame.

Zone (Track by Zone only)

specifies which cell zone this reference frame will track.

Motion (User Defined Only)

allows you to specify a motion for this reference frame (accomplished in the Motion tab.

Linear Velocity (Motion tab)

is the linear velocity with respect to the parent reference frame orientation.

Rotational Velocity (Motion tab)

is the rotational velocity with respect to the parent reference frame orientation.

Rotation Axis

is the axis about which the rotational velocity will be applied.

Origin

specifies the origin of the reference frame.

Axis- Orientation

specifies the orientation of the selected axis.

specifies the orientation of the second axis. By default Fluent does this automatically, however you can

disable Automatic and specify the orientation manually.

Current State (tab)

shows you the current origin and axes directions of the reference frame with respect to the global reference

frame.

The Region Adaption dialog box allows you to mark or refine cells inside or outside a specified region

defined by text or mouse input. This dialog box is only available if you have used the following text

command: mesh/adapt/revert-to-R19.-user-interface; note that if you revert the user

interface, you cannot undo it in the current session, and some functionality is no longer available.

Domain → Adapt → Mark/Adapt Cells → Region...

Controls

Options

contains radio buttons that control whether the cells inside or outside the region are marked for refinement.

Inside

enables the marking of cells with centroids that are within the region.

Outside

enables the marking of cells with centroids that are outside the region.

Shapes

contains radio buttons that control the type of region.

Hex/Quad

defines a hexahedral region in 3D or a rectangular region in 2D.The appropriate button will appear

for the solver you are using.

Sphere/Circle

defines a spherical region in 3D or a circular region in 2D.The appropriate button will appear for the

solver you are using.

Cylinder

defines a cylindrical region in 3D or a rectangular region in 2D.

Manage...

Input Coordinates

defines the extent of the selected region.The appearance of this box changes depending on the type of

region selected.

If the region selected is a hexahedron or quadrilateral, you will specify the minimum and maximum

coordinates defining the box. (The Radius real number field will not be active.)

X Min,Y Min, Z Min

define the coordinates of the minimum point defining the hexahedron or rectangle. For quadrilaterals,

the Z Min real entry field will not be active.

X Max,Y Max, Z Max

define the coordinates of the maximum point defining the hexahedron or rectangle. For quadrilaterals,

the Z Max real entry field will not be active.

If the region selected is a sphere or circle, you will specify the coordinates of the sphere’s center

and its radius. (The maximum coordinate real number fields will not be active.)

X Center,Y Center, Z Center

are the coordinates of the centroid of the sphere or circle. For circles, the Z Center real entry field will

not be active.

Radius

is the radius of the sphere or circle.

If the region selected is a cylinder, you will specify the minimum and maximum coordinates defining

the cylinder axis, as well as the radius of the cylinder.

X-Axis Min,Y-Axis Min, Z-Axis Min

define the coordinates of the minimum point defining the cylinder axis. For 2D cases, the Z-Axis Min

real entry field will not be active.

X-Axis Max,Y-Axis Max, Z-Axis Max

define the coordinates of the maximum point defining the cylinder axis. For 2D cases, the Z-Axis Max

Radius

is the radius of the cylinder. (In 2D, this will be the width of the resulting rectangle.)

allows you to select specify coordinates with the mouse. If one of the mouse buttons is defined as a mouse

probe, you may select the input coordinates from a display of the mesh or solution field. For more inform-

ation on mouse buttons, refer to Controlling the Mouse Button Functions (p. ). After you select the

points, the values will be loaded automatically into the appropriate real number field.You have the option

of editing these values before marking or adapting.The order of input for defining a hexahedron (rectangle)

is insignificant, but the order of input for the sphere (circle) has significance. First, you select the location

of the centroid.Then you select a point that lies on the sphere, that is, a point that is one radius away

from the centroid.

Adapt

adapts the mesh based on the region defined and the in/out option.

Mark

marks the cells to be refined based on the region defined and the in/out option.This command produces

an adaption register.

The Replace Cell Zone dialog box allows you to replace a single cell zone or multiple zones. See Re-

placing Zones (p. ) for details.

Controls

Case/Mesh File

allows you to specify a mesh file from which you want to replace the zone.

Existing Zones

contains a list of cell zones from which you can select the zone to be replaced.

Replace with

contains a list of cell zones from which you can select the zone to replace the zone selected in Existing

Interpolate Data

allows you to enable/disable data interpolation if data already exists.

Replace

replaces the selected cell zone.

Solution → Reports → Definitions → Edit...

For information on creating report definitions, see Monitoring and Reporting Solution Data (p. ).

Controls

lists all of the existing report definitions.

New

defined).

Edit...

allows you to edit the properties of the selected report definition.

Delete

deletes the selected report definition.

Compute

computes the value of the selected report definition and prints to the console.

creates an output parameter for the selected report definition(s) with the name <report definition

name>-op.

Used In

lists the report files and report plots that contain the selected report definition.

Edit...

opens the report file/plot dialog box for the report file/plot selected in the Used In list.

Report Definition Properties

Edit...

displays the properties of the selected report definition in the Report Definition list.

Report File Definitions...

opens the Report File Definitions Dialog Box (p. ).

Report Plot Definitions

opens the Report Plot Definitions Dialog Box (p. ).

Controls

lists all of the existing report files.

New...

opens the New Report File Dialog Box (p. ).

Edit...

allows you to edit the properties of the selected report file in the Edit Report File Dialog Box (p. ).

Delete

deletes the selected report file.

Activate

activates the selected (previously deactivated) report file for writing during the solution calculation.

deactivates the writing of the selected report file during the solution calculation.

lists the report definitions included in the selected report file.

Report File Properties

lists the properties of the selected report file.

Controls

lists all of the existing report plots.

New...

opens the New Report Plot Dialog Box (p. ).

Edit...

allows you to edit the properties of the selected report plot in the Edit Report Plot Dialog Box (p. ).

Delete

deletes the selected report plot.

Activate

activates the selected (previously deactivated) report plot for plotting during the solution calculation.

deactivates the plotting of the selected report plot during the solution calculation.

lists the report definitions included in the selected report plot.

Report Plot Properties

lists the properties of the selected report plot.

You can use the Residual Monitors dialog box to control the residual information that Fluent reports.

See Monitoring Residuals (p. ) for details about the items below.

Solution → Reports → Residuals...

Controls

Options

selects any combination of the following methods for reporting residuals. See Printing and Plotting Re-

siduals (p. ) for details.

specifies whether or not to print residuals in the text window after each iteration.

Plot

specifies whether or not to plot residuals in the graphics window (with the window ID set in Window)

after each iteration. See Plot Parameters (p. ) for details.

Window

sets the window ID in which the plot will be drawn.When ANSYS Fluent is iterating, the active

graphics window is temporarily set to this window to update the residual plot, and then returned to

its previous value.Thus, the residual plot can be maintained in a separate window that does not in-

terfere with other graphical postprocessing.

Iterations to Plot

is the number of history points to display on the residual plot.

Axes...

opens the Axes Dialog Box (p. ), which allows you to modify the attributes of the axes.

Curves...

opens the Curves Dialog Box (p. ), which allows you to modify the attributes of the residual curves.

Iteration to Store

sets the number of residual history points to be stored in the data file. Due to the compaction algorithm

used, saving  points does not result in just the last  iterations being saved; the history reaches

back quite a bit further than that, but does not save a point at every iteration. Further back in the iteration

history, the spacing between saved iterations grows larger. See Storing Residual History Points (p. )

Residual Values

controls the normalization and scaling of residuals. See Controlling Normalization and Scaling (p. ) for

details.

Normalize

specifies whether or not to normalize the printed or plotted residual for each variable by the value

indicated as the Normalization Factor for that variable.The default Normalization Factor is the

maximum residual value after the first  iterations.

This option is off by default.

sets the number of iterations for which ANSYS Fluent will search for the largest residual to normalize

by. (If the Normalize option is turned off, this item will not be editable.)

Scale

specifies whether or not to print or plot scaled residuals for each variable.This option is on by default.

Compute Local Scale

computes and stores both the locally and globally scaled residuals from subsequent iterations, for

the purpose of reporting.You will select the type of residual scaling form the Reporting Option drop-

down list. See Definition of Residuals for the Pressure-Based Solver (p. ) and Definition of Residuals

for the Density-Based Solver (p. ) for more information.

Reporting Option

gives you the choice of plotting or printing to the console the global scaling or local scaling of re-

siduals.

siduals.

consists of four options that are available for checking an equation for convergence.

absolute

is the default and is available for steady-state cases.The residual (scaled and/or normalized) of an

equation at an iteration is compared with a user-specified value. If the residual is less than the user-

specified value, that equation is deemed to have converged for a time step.

relative

is where the residual of an equation at an iteration of a time step is compared with the residual at

the start of the time step. If the ratio of the two residuals is less than a user-specified value, that

equation is deemed to have converged for a time step.

is where either the absolute convergence criterion or the relative convergence criterion is met. At

that point, the equation is considered converged.

none

is used to disable convergence checking.

Convergence Conditions...

opens the Convergence Conditions Dialog Box (p. ).

Residual

indicates the name of each variable for which residual information is available.

Monitor

indicates whether or not the residuals for each variable are to be monitored.You can toggle monitoring

on and off for each variable by turning the corresponding check box in the Monitor list on or off.

Normalization Factor

shows the normalization factor for each variable.The default is the maximum residual value after the first

iterations.To set this value manually, enter a new value in the corresponding Normalization Factor

field.This list will not appear if the Normalize option is turned off.

indicates whether or not the convergence of each variable is to be monitored. If convergence is being

monitored, the solution will stop automatically when each variable meets its specified convergence cri-

terion.You can check convergence only for variables for which you are monitoring residuals.You can

toggle convergence checking on and off for each variable by turning the corresponding check box in the

Check Convergence list on or off.

Absolute Criteria, Relative Criteria

shows the residual value for which the solution of each variable will be considered to be converged.To

set this value manually, enter a new value in the corresponding Absolute Criteria/Relative Criteria field.

Plot

displays the current residual history plot.

Renormalize

sets the normalization factors to the maximum values in the residual histories. Renormalize should be

used to renormalize the residual plot in cases where the maximum residuals occur sometime after the

first five iterations.

The Rotate Mesh dialog box allows you to rotate the mesh about the required axis and rotation origin

by specifying the angle of rotation. See Rotating the Mesh (p. ) for details.

Controls

Rotation Angle

is the angle with which you want to rotate the mesh.You can enter a positive or negative real number.

Rotation Origin

defines the new origin for the mesh rotation.

defines the axis about which you want to rotate the mesh.

Rotate

adds the specified rotation parameters to the appropriate Cartesian coordinate of every node in the mesh.

The S2S Information dialog box allows you to report values of the view factor and radiation emitted

from one zone to any other zone. See Reporting Radiation in the S2S Model (p. ) for details about

the items below.

Controls

contains items for which information is available for reporting.

turns on the computation of view factors from one zone to the other.

turns on the computation of the incident radiation from one zone to the other.

Boundary Types

contains a selectable list of types of boundary zones. If you select (or deselect) an item in this list, all zones

of that type will be selected (or deselected) automatically in the From and To lists.

From

contains a selectable list of boundary zones for which you would like data reported from the selected

zone.

To

contains a selectable list of boundary zones for which you would like data reported to the selected zone.

Compute

computes the view factors and/or incident radiation on the selected zones.

Write...

opens The Select File Dialog Box (p. ), which you can use to save the data as an S2S Info File (.sif

format).

Write...

format).

The Separate Cell Zones dialog box allows you to separate a single cell zone into multiple zones of

the same type. See Separating Zones (p. ) for details.

Controls

Options

specifies the method on which the cell-zone separation is to be based.

Mark

indicates that the cell zone is to be separated based on the marks stored in cell registers.

Region

indicates that the cell zone is to be separated into two or more contiguous regions based on an in-

ternal boundary within the original zone.

Registers

contains a list of defined cell registers. If you are separating the cell zone by mark, select the cell

register to be used in the Registers list. When the separation is performed, cells that are marked

will be placed into a new zone.

Zones

contains a list of cell zones from which you can select the zone to be separated.

Separate

separates the selected cell zone based on the specified parameters.

Report

reports what the result of the separation will be without actually separating the cell zone.

The Separate Face Zones dialog box allows you to separate a single face zone into multiple zones of

Controls

Options

specifies the method on which the face separation is to be based.

Angle

indicates that the face zone is to be separated based on significant angle (specified in the Angle field).

Face

Options

Angle

Face

indicates that the face zone is to be separated by putting each face in the zone into its own zone.

Mark

indicates that the face zone is to be separated based on the marks stored in cell registers.

Region

indicates that the face zone is to be separated based on contiguous regions.

Registers

contains a list of defined cell registers. If you are separating faces by mark, select the cell register

to be used in the Registers list. When the separation is performed, all faces of cells that are marked

will be placed into a new face zone.

Zones

contains a list of face zones from which you can select the zone to be separated.

Angle

specifies the significant angle to be used when you separate a face zone based on angle. Faces with

normal vectors that differ by an angle greater than or equal to the specified significant angle will be

placed in different zones when the separation occurs.

Separate

separates the selected face zone based on the specified parameters.

Report

reports what the result of the separation will be without actually separating the face zone.

The Set Injection Properties dialog box allows you to define the properties of an existing discrete-

phase injection (which was created in the Injections Dialog Box (p. )). See Defining Injection Proper-

ties (p. ) for details about the items listed in this section.

The Set Injection Properties dialog box is opened from the Injections Dialog Box (p. ).

Controls

Injection Name

sets the name of the injection.

Injection Type

Controls

contains a drop-down list of the available injection types: single, group, cone, surface, plain-orifice-

atomizer, pressure-swirl-atomizer, air-blast-atomizer, flat-fan-atomizer, effervescent-atomizer, and

file. (cone is not available in 2D.) These choices are described in Injection Types (p. ).

Number of Streams

indicates the number of particle streams in a group, cone, or any of the atomizer injections. (This item

will not appear for single, surface, or file injections.)

Release From Surfaces

indicates the surface from which the particles in a surface injection will be released. (This item will appear

only for a surface injection.)

specifies the particle type as Massless, Inert, Droplet, Combusting, or Multicomponent.These types

are described in Particle Types (p. ).

Laws

(not for massless particles) contains inputs for customized particle laws.

Custom

enables the specification of customized particle laws and opens the Custom Laws Dialog Box (p. ).

Material

(not for massless particles) indicates the material for the particles. If this is the first time you have created

a particle of this type, you can choose from all of the materials by copying them from the database or

creating them from scratch, as discussed in Setting Discrete-Phase Physical Properties (p. ) and described

in detail in Using the Create/Edit Materials Dialog Box (p. ).

Diameter Distribution

(not for massless particles) allows you to change from the default linear interpolation method used to

determine the size of the particles in a group injection, or the default uniform method used to determine

the size of the particles in a surface injection, to the rosin-rammler or rosin-rammler-logarithmic

method.The Rosin-Rammler method for determining the range of diameters is described in Using the

Rosin-Rammler Diameter Distribution Method (p. ).

Evaporating Species

(for droplet particles) specifies the gas-phase species created by the vaporization and boiling laws (laws

and ).

Devolatilizing Species

(for combusting particles) specifies the gas-phase species created by the devolatilization law (law ).

This item will not appear for two-mixture-fraction non-premixed combustion calculations.

Devolatilizing Stream

(for combusting particles) specifies the destination stream for the gas-phase species created by the de-

volatilization law (law ).

This item will appear only for two-mixture-fraction non-premixed combustion calculations.

Oxidizing Species

(for combusting particles) specifies the gas phase species that participates in the surface char combustion

reaction (law ).

Product Species

(for combusting particles) specifies the gas-phase species created by the surface char combustion reaction

(law ).

Product Stream

(for combusting particles) specifies the destination stream for the gas-phase species created by the surface

char combustion reaction (law ).

Discrete Phase Domain

is available when using the Dense Discrete Phase Model, described in Including the Dense Discrete

Phase Model (p. ).

is available when using the DEM Collision model, described in Modeling Collision Using the DEM Mod-

el (p. ).

Point Properties

displays the inputs for the point properties for the injection (for example, position, velocity, diameter,

temperature, mass flow rate, and stagger options).These inputs are described for each injection type in

Point Properties for Single Injections (p. ) – Point Properties for Effervescent Atomizer Injections (p. ).

Stagger Options

allows you to set the stagger options:

Stagger Positions

enables injection-specific spatial staggering of the particles.

Stagger Radius

specifies the region from which particles are released.This item is available only for non-atomizer

injections.

First Point

specifies the first point properties for the injection.This item appears only for group injections.

Last Point

specifies the last point properties for the injection.This item appears only for group injections.

Update Injection Display

applies the current point property settings to the injection graphics windows so that you can preview

the effect of modified settings before saving the injection.This item is not available for surface, file,

and condensate injection types.

displays the inputs for injection-specific physics models.

Drag Parameters

allows the setting of the drag law used in calculating the force balance on the particles. See Particle

Force Balance in the Theory Guide for details on the items below.

Drag Law

is a drop-down list containing the available choices for the drag law:

spherical

assumes that the particles are smooth spheres.

nonspherical

assumes that the particles are not spheres, but are all identically shaped.The shape is specified

by the Shape Factor.

Stokes-Cunningham

is for use with sub-micron particles. A Cunningham Correction is added to Stokes’ drag law

to determine the drag.

high-Mach-number

is similar to the spherical law with corrections to account for a particle Mach number greater

than . or a particle Reynolds number greater than .

Ishii-Zuber

is used in gas-liquid flows.This drag law is only available if the magnitude and direction of

the gravity vector are specified in the Operating Conditions dialog box. See Ishii-Zuber Drag

Model in the Fluent Theory Guide for details.

Grace

the gravity vector are specified in the Operating Conditions dialog box. See Grace Drag

dynamic-drag

accounts for the effects of droplet distortion.This drag law is available only when one of the

droplet breakup models is used in conjunction with unsteady tracking. See Dynamic Drag

Model Theory in the Theory Guide for details.

Shape Factor

specifies the shape of the particles when nonspherical is selected as the Drag Law (  in

Equation . in the Theory Guide). It is the ratio of the surface area of a sphere having the

same volume as the particle to the actual surface area of the particle.The shape factor value

cannot be greater than .

Cunningham Correction

(

in Equation . in the Theory Guide) is used with Stokes’ drag law to determine the

force acting on the particles when the particles are sub-micron size. It appears when Stokes-

Cunningham is selected as the Drag Law.

Particle Rotation

contains settings for the modeling of particle rotation when the Enable Rotation check box is selected

(see Wall-Particle Reflection Model Theory in the Fluent Theory Guide).

Rotational Drag Law

is a drop-down list of available rotational drag law models:

uses Equation . in the Fluent Theory Guide to calculate the rotational drag coefficient

.

none

implies zero torque, that is, it excludes the influence of the fluid on the rotational particle

motion.

Magnus Lift Law

is a drop-down list of available Magnus lift law models:

uses Oesterle and Bui Dinh’s formulation (Equation . in the Fluent Theory Guide).

is based on the particle spin rate (Equation . in the Fluent Theory Guide).

uses a linear dependence of the rotational lift coefficient

on the spin rate (Equation .

in the Fluent Theory Guide).

none

implies that the Magnus lift will not be included in your simulation.

Brownian Motion

enables the incorporation of the effects of Brownian motion.This option is available only when the

Energy equation is enabled (in the Models group) and the Stokes-Cunningham drag law is selected

from the Drag Law drop-down list. See Brownian Force in the Theory Guide for details.

Breakup

contains parameters that control droplet breakup and collision. (This section of the dialog box appears

only if Unsteady Tracking is enabled in the Discrete Phase Model Dialog Box (p. ).)

Enable Breakup

enables breakup for this injection.

Breakup Model

is a drop-down list containing parameters that control droplet breakup. (This item appears only

if Enable Breakup is selected.)

TAB

enables the Taylor Analogy Breakup (TAB) model, which is applicable to many engineering

sprays.This method is based upon Taylor’s analogy between an oscillating and distorting

droplet and a spring mass system. See Taylor Analogy Breakup (TAB) Model in the Theory

For the TAB model, you must specify the following constants:

y0

Breakup Parcels

is the number of child parcels the droplet is split into, as described in Velocity of Child

Droplets in the Theory Guide.

Wave

enables the Wave breakup model, which considers the breakup of the injected liquid to be

induced by the relative velocity between the gas and liquid phases. See Wave Breakup Model

For the Wave model, you must specify the following constants:

B0

B1

KHRT

enables the Kelvin-Helmholtz Rayleigh-Taylor breakup model, which considers the two com-

B1

KHRT

peting effects of aerodynamic breakup and instabilities due to droplet acceleration. See KHRT

Breakup Model in the Theory Guide for details.

For the KHRT model, you must specify the following constants:

B0

B1

Ctau

CRT

CL

SSD

enables the stochastic secondary droplet breakup model, where the probability of breakup

is independent of the parent droplet size and the secondary droplet size is sampled from an

analytical solution of the Fokker-Planck equation for the probability distribution. See

Stochastic Secondary Droplet (SSD) Model in the Theory Guide for details.

For the SSD model, you must specify the following constants:

Critical We

is the critical Weber number in Equation . in the Theory Guide.

Core B1

is B in Equation . in the Theory Guide.

Target Np

is the average number in parcels for daughter parcels.

Xi

is

Madabhushi

Enables the Madabhushi breakup model.This model is available only with single, group, or

cone (solid cone) injections. Solid cone injection is recommended. For more information about

the Madabhushi breakup model, see Madabhushi Breakup Model in the Fluent Theory Guide.

For the Madabhushi model, you must specify the following constants:

B0

in Equation . in the Theory Guide. The recommended value

is ..

B0

is ..

B1

is .

Jet Diameter

is the nozzle orifice exit diameter.

Ligament Factor

Adjusts the diameter of the child droplets arising from the column breakup mech-

anism

C0

is the column breakup time constant. The value recommended for the Madabhushi

breakup model is ..

displays the inputs for stochastic tracking and cloud tracking.

Stochastic Tracking

controls the stochastic tracking for turbulent flows. Stochastic tracking includes the effect of turbulent

velocity fluctuations on the particle trajectories using the DRW model described in Stochastic Tracking

in the Theory Guide. See Stochastic Tracking (p. ) for details about the items below.

Discrete Random Walk Model

includes the effect of instantaneous turbulent velocity formulations on the particle trajectories

through stochastic method.

Random Eddy Lifetime

specifies that the characteristic lifetime of the eddy is to be random.

Number of Tries

controls the inclusion of turbulent velocity fluctuations.

An input of  or greater tells ANSYS Fluent to include turbulent velocity fluctuations in the

particle force balance.

is

in Equation . in the Theory Guide.The default is . ; if you use the RSM, a value of .

is recommended.

Cloud Tracking

incorporates the effects of turbulent dispersion on the injection. For details on the following items,

see Particle Cloud Tracking in the Theory Guide and Cloud Tracking (p. ).

Cloud Model

enables particle cloud tracking.

Min. Cloud Diameter

specifies the diameter of the cloud in which the particles enter the domain.

Max. Cloud Diameter

specifies the maximum allowed cloud diameter.

Parcel

displays the inputs for controlling the discrete phase parcels.

Parcel Definitions

contains settings for how parcels are defined

Parcel Release Method

specifies the method for releasing parcels. Available settings are standard, constant-number,

constant-mass, and constant-diameter. See Steady/Transient Treatment of Particles (p. ) for

details about these settings.

displays the inputs for the wet combustion model.

Wet Combustion Model

allows the combusting particles to include an evaporating/boiling material.

Liquid Material

contains a drop-down list of liquid materials that can be chosen as the evaporating/boiling material

to be included with the combusting particles.

sets the volume fraction of the liquid present in the particle.

displays the inputs for Multicomponent for use in the definition of the particle injection. For details on

the following items, see Vapor Liquid Equilibrium Theory in the Theory Guide.

Multicomponent Settings

contains the multicomponent injections.

Component

specifies the component that is a part of the multicomponent species.

specifies the mass fraction of the component in a multicomponent species.

specifies the gas-phase species to be evaporated.

Evaporating Stream

specifies the source stream from which the species will be evaporated.

UDF

UDF

displays the inputs for User-Defined Functions for use in the definition of the particle injection. For details

about user-defined functions, see the separate Fluent Customization Manual.

contains a drop-down list of available user-defined functions.The UDF that you choose will be used

to modify the injection properties at the time the particles are injected into the domain.

Heat/Mass Transfer

allows you to select the user-defined function that defines the heat or mass transfer.

Multiple Reactions

displays the inputs for Multiple Surface Reactions. See Particle Surface Reactions (p. ) for details about

this model.

specify the combustible fraction of the combusting particle if you have defined more than one particle

surface species. See Using the Multiple Surface Reactions Model for Discrete-Phase Particle Combus-

File...

opens The Select File Dialog Box (p. ), in which you can select a file containing the injection definition

(when file is selected as the Injection Type).

The Set Multiple Injection Properties dialog box allows you to set properties that are common to

multiple injections. See Defining Properties Common to More than One Injection (p. ) for details

The Set Multiple Injection Properties dialog box is opened from the Injections Dialog Box (p. ).

Controls

Injections Setup

Controls

contains a list of the categories of injection properties that you can set for the injections in the Injections

list.These categories correspond to the categories of inputs in the Set Injection Properties Dialog

Box (p. ).When you select an item in the Injections Setup list, the dialog box will expand to show the

relevant inputs, which are the same as those in the Set Injection Properties dialog box.

displays an informational list of the injections for which you are setting common properties.These are

the injections that you selected in the Injections Dialog Box (p. ).

The Shell Conduction Layers dialog box allows you to define the shell conduction settings for either

a single Wall dialog box or all of the walls selected in the Shell Conduction Zones list of the Shell

Conduction Manager Dialog Box (p. ). See Shell Conduction (p. ) and Managing Shell Conduction

Walls (p. ) for details about the items below.

The Shell Conduction Layers dialog box is opened from either the Wall Dialog Box (p. ) or the

Controls

Number of Shell Conduction Layers

allows you to define the number of layers that make up the wall(s).

Layer , Layer ...

allows you to define the settings for each layer. Note that Layer  refers to the layer closest to the fluid

/ solid adjacent to the wall zone, and layers with higher numbers are further away.

Thickness

sets the thickness of the layer for the calculation of the shell thermal resistance. Each layer must have

Thickness

a nonzero thickness

sets the material type for the layer.The conductivity of the material is used for the calculation of shell

thermal resistance. Materials are defined using the Materials Task Page (p. ).

sets the rate of heat generation in the layer. Note that you have the option of defining the heat gen-

eration rate using a user-defined function (UDF) that utilizes the DEFINE_PROFILE macro; for more

information on creating and using user-defined functions, see the Fluent Customization Manual.

The Shell Conduction Manager dialog box allows you to manage, define, and display shell conduction

zones all in one location. See Managing Shell Conduction Walls (p. ) for details about using the

Shell Conduction Manager dialog box.

Controls

Select Zones

contains the list of Shell Conduction Zones and Wall Zones.

Shell Conduction Zones

contains a list of zones with shell conduction enabled.

Wall Zones

contains a list of zones without shell conduction.

,

disables and enables shell conduction for a selected zone, respectively.

Enable saving shell zones to case file

enables Fluent to automatically writes shell zones into .cas files.

displays the selected walls in the graphics window. Note that you can select walls with or without

shell conduction.The zones will be displayed with different colors depending on the option selected

in Mesh Colors Dialog Box (p. ) (accessible from the Mesh Display Dialog Box (p. )).

opens the Shell Conduction Layers Dialog Box (p. ), where you can define the shell properties of

the walls selected in the Shell Conduction Zones list.

Read...

allows you to define your shell conduction settings by reading a CSV file.

Write...

allows you to write your saved shell conduction settings to a CSV file.

The Structural Point Surface dialog box allows you to interactively create structural point surfaces

(surfaces containing a single data point). See Structural Point Surfaces (p. ) for details about the

Controls

Options

feature.

Point Tool

Reset

Create

Manage...

sizes.

Create

Manage...

sizes.

The Surface Meshes dialog box allows you to read the surface meshes in ANSYS Fluent (See Reading

Surface Mesh Files (p. ) for details on reading surface meshes.)

The Surface Meshes dialog box is opened from the Geometry Based Adaption Dialog Box (p. ).

Controls

Surfaces

contains a list of the surfaces available in the surface mesh you read.

You can select/deselect the surfaces listed under Surfaces.

Read...

opens the Select File dialog box in which you can select the surface mesh you want to read.

Delete

allows you to delete the selected surfaces under Surfaces area.

Display

allows you to display the selected surfaces under Surfaces.

Controls

Options

Per Surface

specifies whether or not the chosen field variable is calculated from all of the selected surfaces com-

bined (default) or individually on each of the selected surfaces.

(optional) To have Fluent calculate a running average for the Surface Report Definition you can

Create

Frequency

op.

selects the integration method used on the selected surfaces.The available report types are the same as

those in the Surface Integrals Dialog Box (p. ). See Surface Integration (p. ) for details.

allows you to specify a vector if you selected Custom Vector Based Flux, Custom Vector Flux or Custom

Vector Weighted Average from the Report Type drop-down list.

contains a list of solution variables that can be monitored on the selected surfaces.This list will not be

available if you select Mass Flow Rate or Volume Flow Rate as the Report Type.

Phase

Phase

Surfaces

contains a selectable list of the current surfaces.

if enabled, this option displays the selected surface(s) in the graphics window.

Point

Line/Rake

Plane

Quadric

Iso-Clip

OK

Compute

computes the value of the report definition at the selected surface(s) and prints to the console.

The Surfaces dialog box allows you to interactively group, rename, and delete surfaces and obtain

information about their components. See Grouping, Editing, Renaming, and Deleting Surfaces (p. )

Controls

Surfaces

contains a list of existing surfaces from which you can select the surface(s) of interest.

Name

displays the name of the selected surface.You can edit the text field to modify the surface name. (If more

than one surface is selected, the name of the first one you selected will be displayed.)

Surface Type

displays the type of surface that is selected (for example, zone-surf if one surface is selected, or Mul-

tiple Surfaces if more than one surface is selected).

Points, 0D Facets, 1D Facets,

and 2D Facets display the number of points and facets in the selected surface. If more than one surface

is selected, the sum over all selected surfaces is displayed for each quantity.

when enabled highlights the surfaces (selected in the Surfaces dialog box) in the graphics window.

ID

displays the ID of the selected surface.You cannot change this value.

UnGroup

ungroups the selected surface.This button is available only if the selected surface was created by Grouping

two or more surfaces together.

Rename

renames the selected surface in Surfaces with the name specified in Name.This button is available when

just one surface is selected. (If two or more surfaces are selected, it becomes the Group button.)

Group

groups two or more selected surfaces and gives the group the name entered in Name.This button replaces

the Rename button when two or more surfaces are selected.

Delete

deletes the selected surface(s).

The Thread Control dialog box allows you to control the maximum number of threads on each machine,

as described in Controlling the Threads (p. ).

Controls

Maximum Number of Spawned Threads

contains a list of options for defining the maximum number of threads on each machine.

specifies that the maximum number of threads on each machine is equal to the number of ANSYS

Fluent node processes on each machine.

specifies that the maximum number of threads on each machine is equal to the number of cores on

the machine. ANSYS Fluent obtains the number of cores from the OS.

specifies that the maximum number of threads that can be spawned on each machine is equal to the

number you provide in the number-entry box below Fixed Number.

The Transform Surface dialog box allows you to create a new data surface by rotating and/or trans-

lating an existing surface, and/or by specifying a constant normal distance from it. See Transforming

Controls

Rotate

contains the transformation parameters for rotation.

About

defines the origin about which the surface is rotated.You will specify a point, and the origin of the

coordinate system for the rotation will be set to the specified point. For example, if you specified the

point (,) in 2D, rotation would be about the  axis anchored at (,).You can either enter the point’s

coordinates in the x,y,z fields or click the Mouse Select button and select a point in the graphics

window using the mouse.

Angles

define the angles about the x, y, and z axes (that is, the axes of the coordinate system with the origin

defined under About) by which the surface is rotated. For 2D problems, you can specify rotation

about the z axis only.

Translate

contains the transformation parameters for translation.

x,y,z

Translate

x,y,z

define the distance by which the surface is translated in each direction.

Iso-Distance

contains the transformation parameters for “isodistancing.”

d

sets the normal distance between the original surface and the transformed surface.

Transform Surface

contains a list of existing surfaces from which you can select the surface to be transformed.The selected

surface will remain unchanged; the transformation will create a new surface.

designates the name of the new surface.The default is the concatenation of the transformation type (that

is, iso-distance, rotate, or translate) and an integer which is the new surface ID.

Create

Manage...

sizes.

The Translate Mesh dialog box allows you to change the origin of the mesh. See Translating the

Mesh (p. ) for details.

Controls

Translation Offsets

contains the desired changes in the mesh coordinates (that is, the desired delta in the axes origin).You

can enter a positive or negative real number.

X,Y,Z

defines the deltas in the ,

, and  directions, in the current units of length.

Translate

adds the specified translation offsets to the appropriate Cartesian coordinate of every node in the mesh.

The Turbo 2D Contours dialog box enables you to display turbomachinery-specific contours of variables

on surfaces of constant pitchwise, spanwise, or meridional coordinates, projected onto a plane. See

Displaying Turbomachinery 2D Contours (p. ) for details.

Controls

Turbo Topology

contains a list of defined topologies. Select from the list to display the values for the selected topology.

Options

Filled

Auto Range

Levels

sets the number of contour levels that are displayed.

Setup

indicates the ID number of the contour setup. For frequently used combinations of contour fields and

options, you can store the information needed to generate the contour plot by specifying a Setup number

and setting up the desired information in the dialog box. See Storing Contour Plot Settings (p. ) for

details.

Min

new value.

Max

new value.

Normalised Spanwise Coordinates ( to )

enables you to specify the coordinate for the spanwise surface you want to create.

Display

Compute

The Turbo Averaged Contours dialog box enables you to display turbomachinery-specific circumfer-

entially averaged contours of variables projected on an -  plane. See Displaying Turbomachinery

Averaged Contours (p. ) for details.

Controls

Options

Controls

Options

Filled

Auto Range

Levels

Setup

details.

Min

new value.

Max

new value.

Domain Min

shows the global minimum value of the scalar field for the entire domain.

Domain Max

new value.

Domain Min

Domain Max

shows the global maximum value of the scalar field for the entire domain.

Display

Compute

The Turbo Averaged XY Plot dialog box enables you to display data in an XY plot format as a function

of either the meridional or the spanwise coordinate. See Generating Averaged XY Plots of Turboma-

chinery Solution Data (p. ) for details.

Controls

Min

shows the minimum value of the scalar field.

Max

shows the maximum value of the scalar field.

enables you to select the coordinate to be used for the  axis of the plot.The choices are Hub to Casing

Distance (spanwise coordinate), and Meridional Distance (meridional coordinate).

Fractional Distance

sets a fractional value ( to ) for either the spanwise Hub to Casing distance or the meridional Inlet to

Outlet distance, depending on your selection for X Axis Function.

enables the file-writing option.When this option is selected, the Plot button will change to Write....

Clicking on the Write... button will open The Select File Dialog Box (p. ), in which you can specify a

name and save a file containing the plot data.The format of this file is described in XY Plot File

Plot

Write...

opens The Select File Dialog Box (p. ), in which you can save the plot data to a file.This button replaces

the Plot button when the Write to File option is turned on.

Compute

calculates the scalar field and updates the Min and Max values.

Axes...

opens the Axes Dialog Box (p. ), which enables you to customize the plot axes.

Curves...

opens the Curves Dialog Box (p. ), which enables you to customize the curves used in the XY plot.

The Turbo Options dialog box enables you to globally set the turbomachinery topology for your

model. See Globally Setting the Turbomachinery Topology (p. ) for details.

Controls

Current Topology

contains a list of predefined turbo topologies.

The Turbo Report dialog box allows you to calculate turbomachinery-specific quantities and integrals.

See Generating Reports of Turbomachinery Data (p. ) for details.

Controls

Inlet/Outlet Data

contains quantities that can be calculated at inlets and outlets.

Averages

allows you to choose between Mass-Weighted and Area-Weighted averages for all applicable

computed quantities.These quantities are calculated for the Inlet and Outlet topologies where ap-

plicable.

plicable.

Mass Flow

is the mass flow rate through a surface as defined in Equation . (p. ).

Swirl Number

is the swirl number as defined in Equation . (p. ).

Average Total Pressure

is the area-averaged or mass-averaged total pressure as defined in Equation . (p. ) or Equa-

Average Total Temperature

is the area-averaged or mass-averaged total temperature as defined in Equation . (p. ) or

Average Radial Flow Angle

is the area-averaged or mass-averaged radial flow angle as defined in Equation . (p. ) or Equa-

Average Theta Flow Angle

is the area-averaged or mass-averaged tangential flow angle as defined in Equation . (p. ) or

Losses

contains the values of loss-related coefficients.

Engr. Passage Loss Coef

is the engineering loss coefficient as defined in Equation . (p. ).

Norm. Passage Loss Coef

is the normalized loss coefficient as defined in Equation . (p. ).

Forces

contains the axial force and the torque on the rotating parts.

Axial Force

is the axial force on the rotating parts as defined in Equation . (p. ).

Torque

is the torque on the rotating parts as defined in Equation . (p. ).

Efficiencies

contains the values of isentropic, polytropic and hydraulic efficiencies.

Isentropic

is the isentropic efficiency for a compressor or a turbine (motor) calculated in the presence of a

compressible working fluid as defined in Equation . (p. ) or Equation . (p. ).

Polytropic

is the polytropic efficiency for a compressor or a turbine (motor) calculated in the presence of a

Hydraulic

is the hydraulic efficiency for a pump or a hydraulic turbine (motor) calculated in the presence of an

incompressible working fluid as defined in Equation . (p. ) or Equation . (p. ).

Compute

starts the calculation of the quantities in all the fields in the Turbo Report dialog box. Note that this

process may take some time for a large problem.

Write...

opens the Select File dialog box, which you can use to save the reported values to a file.

The Turbo Topology dialog box allows you to define the topology for a turbomachinery application,

so that you can use the turbomachinery-specific postprocessing features described in Turbomachinery

Postprocessing (p. ). See Defining the Turbomachinery Topology (p. ) for details about the items

below.

Controls

Turbo Topology Name

specifies the name of the new topology.

contains radio buttons for the topology boundaries to be defined.

Hub

specifies the definition for the wall zone(s) forming the lower boundary of the flow passage (generally

toward the axis of rotation of the machine).

Casing

specifies the definition of the wall zone(s) forming the upper boundary of the flow passage (away

from the axis of rotation of the machine).

specifies the definition of the periodic boundary zone(s) on the circumferential boundaries of the

flow passage.

Theta Min,Theta Max

specify the definition of the wall zones at the minimum and maximum angular ( ) positions on a cir-

cumferential boundary.

Inlet

specifies the definition of the inlet zone(s) through which the flow enters the passage.

Outlet

specifies the definition of the outlet zone(s) through which the flow exits the passage.

Blade

specifies the definition of the wall zone(s) that defines the blade(s) (if any). Note that these zones

cannot be attached to the circumferential boundaries. For this situation, use Theta Min and Theta

Max to define the blade.

Surfaces

contains a selectable list of the available surfaces, from which you can select the surface(s) that represent

the boundary selected under Boundaries.

Define

defines the new topology. If you have selected an existing topology the Define button is replaced by the

Modify button.

Display

draws the defined topology in the active graphics window.

The UDF Library Manager dialog box allows you to load/unload the user-defined function libraries.

Controls

UDF Libraries

lists the user-defined function libraries that are loaded in ANSYS Fluent.

specifies the name of the library to be loaded/unloaded.

Load

Unload

unloads the specified library.

Load

Unload

The User-Defined Fan Model dialog box allows you to periodically regenerate a profile file that can

swirling components of velocity generated by the fan. See User-Defined Fan Model (p. ) for details

about this feature and how to use this dialog box.

Controls

Fan Zones

contains a list from which you can select the fan zone(s) on which your executable will operate.

Iteration Update Interval

specifies how often the executable will be called on to update the fan profile file.

Output Profile Points

specifies the number of points in the profile file to be written by ANSYS Fluent.

External Command Name

specifies the name of the executable.

The User-Defined Function Hooks dialog box allows you to specify user-defined functions (UDFs)

connected to a number of models and procedures in ANSYS Fluent. See the separate Fluent Custom-

Important

You can hook multiple UDFs to the following functions:

Controls

Adjust

Execute At End

Read Case

Write Case

Read Data

Write Data

Execute at Exit

Controls

selects a UDF that is called immediately after you initialize your flow field.

Adjust

selects a UDF that is called at the beginning of an iteration before solution of velocities, pressure, and

other quantities begins.

Adjust

selects a UDF that is called at the end of an iteration or time-step.

Read Case

selects a UDF that defines a customized section that is to be read from the case file.

Write Case

selects a UDF that defines a customized section that is to be written to the case file.

Read Data

selects a UDF that defines a customized section that is to be read from the data file.

Write Data

selects a UDF that defines a customized section that is to be written to the data file.

selects a UDF that is called when exiting an ANSYS Fluent session.

Wall Heat Flux

selects a UDF that modifies the way that the solver computes the heat flux between a wall and the

neighboring fluid cells.

Net Reaction Rate

selects a UDF that defines the net reaction rate.

Volume Reaction Rate

selects a UDF that defines a volumetric reaction rate.

Surface Reaction Rate

selects a UDF that defines a surface reaction rate.

Particle Reaction Rate

selects a UDF that defines a particle reaction rate.

Turbulent Premixed Source

selects a UDF that defines the turbulent flame speed and source term for the premixed or partially premixed

Chemistry Step

selects a UDF that defines the chemistry step function.

Spray Collide

selects a UDF that defines the spray collide function.

Cavitation Mass Rate

selects a UDF that defines the cavitation rate.

DO Source

selects a UDF that defines the discrete ordinate source function.

DO Diffuse Reflectivity

selects a UDF that defines the diffuse reflectivity function for the DO radiation model.

DO Specular Reflectivity

selects a UDF that defines the specular reflectivity function for the DO radiation model.

Emissivity Weighting Factor

selects a UDF that defines the emissivity weighting factor for the non-gray DO radiation model or the

non-gray P- radiation model.

Thickened Flame Model Parameters

selects a UDF that defines the parameters for the Thickened Flame Model.

The User-Defined Memory dialog box allows you to allocate memory for user-defined storage variables.

Controls

Number of User-Defined Memory Locations

specifies the number of memory locations to be allocated.

Number of User-Defined Node Memory Locations

specifies the number of node memory locations to be allocated.

Important

For postprocessing User-Defined Memory in CFD-Post, the ANSYS Fluent user must select

the UDM quantities using the Data File Quantities option and subsequently write the data

file to postprocess the quantities in ANSYS Fluent. Alternatively, you have the option of

exporting the desired quantities to a .cdat file. This will ensure that all the UDM quantities

are available for postprocessing in CFD-Post. Refer to the ANSYS CFD-Post manual for more

Solution → Reports → Definitions → New → User Defined...

or

Controls

Function

drop-down list where you can select the function that you loaded for this report definition.

Controls

Function

(optional) To have Fluent calculate a running average for the User Defined Report Definition you can

Create

Frequency

op.

The User-Defined Scalars dialog box allows you to include user-defined scalar transport equations in

op.

your calculation. See User-Defined Scalar (UDS) Transport Equations (p. ) for details.

User Defined → User Defined → Scalars...

Controls

Number of User-Defined Scalars

specifies how many additional scalar transport equations you would like to include in the calculation.

when enabled allows you to include the diffusion term in the UDS transport equation for all inflow and

User-Defined Scalars Options

contains settings that define the scalar transport equation.

UDS Index

when set to  marks the first user-defined scalar equation.

Solution Zones

specifies in which zone the scalar equation will be solved: all fluid zones, all solid zones, all zones

(fluid and solid) or selected zones.

Flux Function

is a drop-down list containing available functions for the convection term of the user-defined scalar

transport equation(s).

none

(the default) indicates that there is no convection term included in the scalar transport equation(s);

that is, you want to solve a Poisson equation instead of a convection/diffusion equation.

indicates that the convection term in the scalar transport equation(s) is equal to the mass flow

rate

.

Note that the none and mass flow rate options will apply to all solved user-defined scalars.

A user-defined flux function must be supplied if a different convective flux is desired for each

user-defined scalar.

Unsteady Function

is a drop-down list containing available functions for the unsteady term of the user-defined scalar

The Vectors dialog box controls the display of vector plots. See Displaying Vectors (p. ) for details

Results → Graphics → Vectors → New...

Controls

is the name for a vector plot definition.You can specify a name or use the default name  vector-id.

This control appears only for vector plot definitions.

Options

contains check buttons that set various display options.

Auto Range

toggles between automatic and manual setting of the range of scalar field values.

controls the display of vectors that have a value outside the range specified by Min and Max.When

on, no vectors are displayed outside the range.When off, vectors are displayed outside the range

using the colors at the top and bottom of the color scale.This option is applicable only when Auto

Range is off. See Specifying the Range of Magnitudes Displayed (p. ) for details.

Auto Scale

enables the scaling of all vectors in the domain such that when the Scale is , there will be minimal

overlap of vectors.

Draw Mesh

Style

selects the style in which the vectors are drawn. Available styles are 3d arrow, 3d arrowhead, cone,

filled-arrow, arrow, harpoon, and headless.

Scale

Style

Scale

sets the factor by which the vectors should be scaled. See Scaling the Vectors (p. ) for details.

Skip

allows you to “thin” or “sample” the vectors that are displayed. See Skipping Vectors (p. ) for details.

Vector Options...

opens the Vector Options Dialog Box (p. ), in which you can set additional options for vector displays.

(This button is not available for vector plot definitions.)

Custom Vectors...

opens the Custom Vectors Dialog Box (p. ), in which you can define your own vector fields.

Vectors of

contains a list from which you can select the vector field to be plotted.

Color by

contains a list from which you can select the scalar field by which the vectors are colored.

Min

shows the value to which the lower end of the color scale is mapped.You can set this value manually if

Auto Range is off.

Max

shows the value to which the upper end of the color scale is mapped.You can set this value manually if

Surfaces

contains a list from which you can select the surfaces on which to display vectors. In 2D, vectors are dis-

played on the entire domain if no surface is selected.

Point

Line/Rake

Plane

Quadric

Line/Rake

Plane

Quadric

Iso-Clip

Display

draws the vectors in the active graphics window.

Compute

plots the vectors in the active graphics window and saves the vector plot definition.This button appears

only for vector plot definitions and replaces the Display button.

The Volume Adaption dialog box allows you to mark or refine cells based on cell volume or change

in cell volume. This dialog box is only available if you have used the following text command:

mesh/adapt/revert-to-R19.-user-interface; note that if you revert the user interface,

you cannot undo it in the current session, and some functionality is no longer available.

Domain → Adapt → Mark/Adapt Cells → Volume...

Controls

Options

allows you to specify that the marking and/or refining is based on volume magnitude or volume change.

Magnitude

enables the marking/refining of cells based on volume magnitude.

Change

enables the marking/refining of cells based on the change in volume.

Min

displays the minimum value of cell volume or cell volume change in the mesh.This value is not editable.

Max

displays the maximum value of cell volume or cell volume change in the mesh.This value is not editable.

Max Volume

defines the threshold value for marking/refining the mesh based on volume magnitude. Cells that have

Max Volume

volumes greater than the threshold are marked for refinement.

Max Volume Change

defines the threshold value for marking/refining the mesh based on the change in volume. Cells with

volume changes that are greater than the threshold value are marked for refinement.

Manage...

Adapt

refines the mesh based on either the maximum volume or the volume change, and the adaption limits.

Mark

marks cells to be refined based on either the maximum volume or the volume change.This command

produces an adaption register.

Compute

calculates the minimum and maximum cell volume or cell volume change and displays them in the Min

and Max real number fields.

Controls

Options

Per Zone

specifies whether or not the chosen field variable is calculated from all of the selected cell zones

combined (default) or individually on each of the selected cell zones.

(optional) To have Fluent calculate a running average for the Volume Report Definition you can

Create

Frequency

op.

contains a list of solution variables that can be monitored on the selected cell zones.This list will not be

available if you select Volume as the Report Type.

Phase

Cell Zones

Phase

Cell Zones

contains a selectable list of the current cell zones.

OK

Compute

The Warning dialog box allows you to specify whether existing dynamic zones and/or mesh interfaces

are deleted when you are using the Merge Zones dialog box to merge multiple zones of the same

type into a single zone (see Merge Zones Dialog Box (p. ) for details). Note that dynamic zones and

mesh interfaces that exist at the time of the merge may be adversely affected by the merge.

The Warning dialog box opens automatically when you click Merge in the Merge Zones Dialog

Box (p. ) if your case has dynamic zones or mesh interfaces.

Controls

Cancel Merging

returns you to the Mesh Zones dialog box when you click OK, without initiating the merge.

Proceed at Your Own Risk

allows the merge to proceed when you click OK, without deleting the existing dynamic zones and mesh

interfaces beforehand.

Proceed After Mesh Manipulation

deletes the existing dynamic zones and/or mesh interfaces (based on the settings in the Mesh Manipu-

lation group box) and then merges the zones when you click OK.

Mesh Manipulation

allows you to specify whether the existing dynamic zones and/or mesh interfaces are deleted prior to the

initiation of the merge.This group box is only available when Proceed After Mesh Manipulation is se-

lected.

Dynamic Zones

specifies whether all existing dynamic zones are deleted prior to the merge.

lected.

specifies whether all existing mesh interfaces are deleted prior to the merge.

Note that selecting keep all from both drop-down lists in the Mesh Manipulation group box is

the equivalent of selecting Proceed at Your Own Risk.

The Yplus/Ystar Adaption dialog box allows you to mark or adapt boundary cells on specified wall

zones based on the non-dimensional

or

parameter. This dialog box is only available if you have

used the following text command: mesh/adapt/revert-to-R19.-user-interface; note

that if you revert the user interface, you cannot undo it in the current session, and some functionality

is no longer available.

Domain → Adapt → Mark/Adapt Cells → Yplus/Ystar...

Controls

Options

Refine

toggles the ability to refine cells or mark cells for refinement.

Coarsen

toggles the ability to coarsen cells or mark cells for coarsening.

Type

contains the check buttons that enable adaption based on

or

.

Yplus

enables

adaption.

Ystar

enables

adaption.

Wall Zones

contains a selectable list of active wall zones. Boundary cells associated with the wall zones you select

will be marked or adapted based on the options, thresholds, and limitations applied in the dialog box.

Min/Max

displays the minimum and maximum cell values of

or

for all cells associated with viscous wall zones.

Note that these values are independent of the wall zones selected.The real number field values are not

editable; they are purely informational.

Min Allowed

designates the threshold value for coarsening the mesh. Cells with

or

values below the minimum

threshold will be marked for coarsening.

Max Allowed

designates the threshold value for refining the mesh. Cells with

or

values above the maximum

threshold will be marked for refinement.

Manage...

Adapt

adapts the mesh based the coarsening and refining toggle buttons, the wall zones selected, the minimum

and maximum

or

allowed, and the adaption limits.

Mark

marks cells to be refined and/or coarsened based on the wall zones selected and the minimum and

maximum

or

allowed in the mesh.This command produces an adaption register.

Compute

computes the minimum and maximum values of

or

on all cells on viscous walls and displays them

in the Min and Max real number fields. Note that these are the extremes for the

or

values of every

cell on a viscous wall, not just the cells associated with the selected zones.

The Zone Surface dialog box allows you to interactively create surfaces from face and cell zones in

the domain. See Zone Surfaces (p. ) for details about the items below.

Controls

Zone

lists zones that you can select for creating zone surfaces.

Surfaces

Controls

Zone

Surfaces

designates the name of the surface to be created.The default is the zone name.

Create

Manage...

sizes.

Appendix A. ANSYS Fluent Model Compatibility

The following tables summarize the compatibility of several ANSYS Fluent model categories:

Multiphase Models (see Modeling Multiphase Flows (p. ))

Moving Domain Models (See Modeling Flows with Moving Reference Frames (p. ))

Turbulence Models (See Modeling Turbulence (p. ))

Combustion Models (See Chapters  Modeling Species Transport and Finite-Rate Chemistry (p. ) – Modeling

Engine Ignition (p. ))

Note that a ✓ indicates that two models are compatible with each other, while the absence of a ✓ in-

dicates that two models are not compatible with each other.

Table : Moving Domain Models vs. Multiphase Models

Mixture

VOF

Eulerian

✓

✓

✓

✓

Sliding Mesh

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

Multiple

✓

✓

✓

✓

Single Reference

Frame

Table : Multiphase Models vs. Turbulence Models

LES

k-omega**

k-epsilon*

Spalart−Allmaras

✓

✓

✓

Eulerian

✓

✓

✓

✓

✓

VOF

✓

✓

✓

✓

✓

Mixture

✓

✓

✓

✓

✓

Discrete

Phase

Table : Combustion Models vs. Multiphase Models

Mixture

VOF

Eulerian

✓

✓

✓

✓

Laminar Finite

Rate

✓

✓

✓

✓

Eddy Dissipation

✓

Concept

✓

Non-Premixed

✓

Premixed

✓

Partially Premixed

Mixture

VOF

Eulerian

✓

✓

✓

✓

Rate

✓

✓

✓

✓

✓

Concept

✓

✓

Premixed

✓

Eulerian PDF only

Composition PDF

Transport

✓

Table : Moving Domain Models vs. Turbulence Models

LES

k-omega**

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

✓

Multiple

Reference

Frame

✓

✓

✓

✓

✓

Single

Reference

Frame

Table : Combustion Models vs. Moving Domain Models

Frame

Multiple Reference

Frame

Mixing

Plane

Sliding

Mesh

✓

✓

✓

✓

Rate

✓

✓

✓

✓

✓

✓

✓

✓

Concept

✓

✓

✓

✓

✓

✓

✓

✓

Premixed

✓

✓

✓

✓

✓

✓

✓

✓

Transport

✓

✓

✓

✓

Table : Combustion Models vs. Turbulence Models

LES

Reynolds

Stress

k-omega**

✓

✓

✓

✓

✓

Rate

✓

✓

✓

✓

Eddy

ANSYS Fluent Model Compatibility

✓

✓

✓

✓

Eddy

Concept

✓

✓

✓

✓

✓

✓

✓

✓

Premixed

✓

✓

✓

✓

Partially

Premixed

✓

✓

✓

✓

PDF Transport

✓

✓

✓

✓

Key:

✓ - compatible

- Includes Standard, RNG, and Realizable k-epsilon models

** - Includes Standard, BSL, and SST k-omega models

Appendix B. ANSYS Fluent File Formats

This appendix provides information about the following:

B.. Case and Data File Formats

B.. Mesh Morpher/Optimizer File Formats

B.. Shell Conduction Settings File Format

B.. 3D Fan Curve File Format

This section describes the contents and formats of ANSYS Fluent case and data files. After discussing

the Guidelines (p. ) and Formatting Conventions in Binary and Formatted Files (p. ), the section

descriptions are grouped according to function:

Grid Sections (p. ) : Creating grids for ANSYS Fluent.

Other (Non-Grid) Case Sections (p. )

Data Sections (p. ) : Importing solutions into another postprocessor.

The case and data files may contain other sections that are intended for internal use only.

B... Guidelines

The ANSYS Fluent case and data files are broken into several sections according to the following

guidelines:

is different for formatted and binary files (Formatting Conventions in Binary and Formatted Files (p. )).

Header information for lists of items is enclosed in separate sets of parentheses preceding the items, and

the items are enclosed in their own parentheses.

B... Formatting Conventions in Binary and Formatted Files

For formatted files, examples of file sections are given in Grid Sections (p. ) and Other (Non-Grid)

Case Sections (p. ). For binary files, the header indices described in this section (for example,  for

binary data (for example,  or  instead of ). The end of the binary data is indicated by

End of Binary Section  or End of Binary Section  before the closing par-

enthesis of the section.

( (  2aad  )(

.

.

.

)

B... Grid Sections

Grid sections are stored in the case file. A grid file is a subset of a case file, containing only those sections

pertaining to the grid. The currently defined grid sections are:

Comment (See Comment (p. ))

Header (See Header (p. ))

Dimensions (See Dimensions (p. ))

Nodes (See Nodes (p. ))

Periodic Shadow Faces (See Periodic Shadow Faces (p. ))

Cells (See Cells (p. ))

Faces (See Faces (p. ))

Face Tree (See Face Tree (p. ))

Cell Tree (See Cell Tree (p. ))

Interface Face Parents (See Interface Face Parents (p. ))

are available as symbols in a Scheme source file (xfile.scm), which is available from ANSYS Inc., or

B.... Comment

Index:

C macro:

optional

Status:

You should precede each long section, or group of related sections, by a comment section explaining

Example:

( (

(relax-mass-flow )

ANSYS Fluent File Formats

(default-coefficient ())

(default-method )

))

B.... Header

Index:

xf-header

XF_HEADER

C macro:

optional

Status:

( (

))

Index:

xf-header

XF_HEADER

C macro:

optional

Status:

example:

( "fluent19.. build-id: ")

The purpose of this section is to identify the program that wrote the file. Although it can appear

anywhere, it is one of the first sections in the file. Additional header sections indicate other programs

that may have been used in generating the file. It provides a history mechanism showing where the

file came from and how it was processed.

B.... Dimensions

Index:

C macro:

optional

Status:

( ND)

where ND is  or . This section is supported as a check that the grid has the appropriate dimension.

B.... Nodes

Index:

xf-node

XF_NODE

C macro:

required

Status:

Format:

x1 y1 z1

x2 y2 z2

.

.

.

))

Case and Data File Formats

If zone-id is zero, this provides the total number of nodes in the grid. first-index will then be one,

last-index will be the total number of nodes in hexadecimal, type is equal to , ND is the dimension-

ality of the grid, and there are no coordinates following (the parentheses for the coordinates are omitted

as well).

For example: ( (  2d5  ))

If zone-id is greater than zero, it indicates the zone to which the nodes belong. first-index and

last-index are the indices of the nodes in the zone, in hexadecimal.The values of last-index in

each zone must be less than or equal to the value in the declaration section. Type is always equal to .

ND is an optional argument that indicates the dimensionality of the node data, where ND is  or

.

If the number of dimensions in the grid is two, as specified by the node header, then only  and

coordinates are present on each line.

The following is an example of a 2D grid:

( (  2d5  )(

.

.

.

))

Because the grid connectivity is composed of integers representing pointers (see Cells and Faces),

using hexadecimal conserves space in the file and provides for faster file input and output. The

header indices are in hexadecimal so that they match the indices in the bodies of the grid connectivity

sections. The zone-id and type are also in hexadecimal for consistency.

B.... Periodic Shadow Faces

Index:

C macro:

required only for grids with periodic boundaries

Status:

boundaries do not have sections of this type. The format of the section is as follows:

f00 f01

f10 f11

f20 f21

.

.

.

))

where

first-index = index of the first periodic face pair in the list

last-index = index of the last periodic face pair in the list

periodic-zone = zone ID of the periodic face zone

shadow-zone = zone ID of the corresponding shadow face zone

These are in hexadecimal format. The indices in the section body (f*) refer to the faces on each of

the periodic boundaries (in hexadecimal), the indices being offsets into the list of faces for the grid.

Note

In this case, first-index and last-index do not refer to face indices. They refer to

indices in the list of periodic pairs.

Example:

( ( 2b a c) (

1f

ad 1c2

.

.

.

))

B.... Cells

Index:

xf-cell

XF_CELL

C macro:

required

Status:

Again, zone-id is zero to indicate that it is a declaration of the total number of cells. If last-index

is zero, then there are no cells in the grid. This is useful when the file contains only a surface mesh

to alert ANSYS Fluent that it cannot be used. In a declaration section, the type has a value of zero

and the element-type is not present.

( (  3e3 ))

It states that there are 3e3 (hexadecimal) =  cells in the grid. This declaration section is required

and must precede the regular cell sections.

mixed

pyramid

wedge

NF

NN

and last-index indicate the range for the particular zone, type indicates whether the cell zone

is an active zone (solid or fluid), or inactive zone (currently only parent cells resulting from hanging

node adaption). Active zones are represented with type=, while inactive zones are represented

with type=.

In the earlier versions of ANSYS Fluent, a distinction was made between solid and fluid zones. This is

now determined by properties (that is, material type).

A type of zero indicates a dead zone and will be skipped by ANSYS Fluent. If a zone is of mixed type

(element-type=), it will have a body that lists the element-type of each cell.

Example:

( (  3d  )(

.

.

.

))

Here, there are 3D (hexadecimal) =  cells in cell zone , of which the first  are triangles, the next

are quadrilaterals, and so on.

B.... Faces

Index:

xf-face

XF_FACE

C macro:

required

Status:

The format for face sections is as follows:

where

The current valid boundary condition types are defined in the following table:

bc-type

interior

wall

symmetry

periodic

mass-flow-inlet, mass-flow-outlet

interface

outflow

axis

symmetry

periodic

interface

outflow

axis

The faces resulting from the intersection of non-conformal grids are placed in a separate face zone,

where a factor of  is added to the bc-type (for example,  is a wall zone).

The current valid face types are defined in the following table:

face-type

mixed

linear

NN

polygonal

faces in the file. Such a section omits the bc-type and is not followed by a body with further inform-

ation.

A nonzero zone-id indicates a regular face section, and will be followed by a body that contains

information about the grid connectivity. Each line of the body will describe one face and will have

the following format:

where,

n* = defining nodes (vertices) of the face

c* = adjacent cells

This is the format for a 3D grid with a triangular face format. The actual number of nodes depends

on the face-type. The order of the cell indices is important, and is determined by the right-hand

rule: if you curl the fingers of your right hand in the order of the nodes, your thumb will point toward

c0.

For 2D grids, n2 is omitted. c1 is determined by the cross product of two vectors,  and . The

vector extends from n0 to n1, whereas the  vector has its origin at n0 and points out of the grid

plane toward the viewer. If you extend your right hand along  and curl your fingers in the direction

of the angle between  and , your thumb will point along

toward c1.

If the face zone is of mixed type (face-type= ) or of polygonal type (face-type= ), each line

of the section body will begin with a reference to the number of nodes that make up that particular

face, and has the following format:

where,

x = the number of nodes (vertices) of the face

nf = the final node of the face

All cells, faces, and nodes have positive indices. If a face has a cell only on one side, then either c0

or c1 is zero. For files containing only a surface mesh, both these values are zero.

For information on face-node connectivity for various cell types in ANSYS Fluent, refer to Face-Node

Connectivity in ANSYS Fluent (p. ).

B.... Face Tree

Index:

C macro:

only for grids with hanging node adaption

Status:

This section indicates the face hierarchy of the grid containing hanging nodes. The format of the

section is as follows:

(

.

.

.

))

where,

face-id0 = index of the first parent face in the section

face-id1 = index of the last parent face in the section

parent-zone-id = ID of the zone containing parent faces

child-zone-id = ID of the zone containing children faces

number-of-kids = the number of children of the parent face

kid-id-n = the face IDs of the children

B.... Cell Tree

Index:

C macro:

Status:

Index:

C macro:

Status:

This section indicates the cell hierarchy of the grid containing hanging nodes. The format of the

(

.

.

.

))

where,

cell-id0 = index of the first parent cell in the section

cell-id1 = index of the last parent cell in the section

parent-zone-id = ID of the zone containing parent cells

child-zone-id = ID of the zone containing children cells

number-of-kids = the number of children of the parent cell

kid-id-n = the cell IDs of the children

B.... Interface Face Parents

Index:

C macro:

only for grids with non-conformal interfaces

Status:

fraction of the original face. Each child will refer to at least one parent. The format of the section is

(

.

.

.

))

where,

face-id0 = index of the first child face in the

section

face-id1 = index of the last child face in the

section

parent-id-* = index of parent faces

If you set up and save a non-conformal mesh in the solution mode of Fluent and then read it using

the meshing mode of Fluent, this section will be skipped; consequently, all the information necessary

to preserve the non-conformal interface will not be maintained. When you switch to or read the mesh

B.... Example Files

B..... Example

Figure : Quadrilateral Mesh (p. ) illustrates a simple quadrilateral mesh with no periodic bound-

aries or hanging nodes.

( "Grid:")

( )

( (   ))

( (  a ))

( (    ))

( (    ))

( (    )(

))

( (    )(

))

( (    )(

))

( (   a )(

))

( ( a a  )(

))

( (    )

(

Figure : Quadrilateral Mesh with Periodic Boundaries (p. ) illustrates a simple quadrilateral mesh

with periodic boundaries but no hanging nodes. In this example, bf9 and bf10 are faces on the

periodic zones.

( )

( "Grid:")

( (   ))

( (  a ))

( (    ))

( (    ))

( (    )(

))

( (    )(

))

( (    )(

))

( (   c )(

))

( ( a a  )(

))

( (   )(

a))

( (    )(

( "Grid:")

( )

( (   ))

( (   ))

( (  d  ))

( (    ))

( (    ))

( (   )(

))

( (    )(

))

( (  b  )(

a

b

))

( ( c f  )(

c

d  ))

( (   a )(

d a  ))

( (    )(

c

b   ))

( (b   1f )(

c   ))

( (a   1f )(

b c  ))

( (   1f )(

b  ))

( (   1f )(

))

( (  b )(

d c))

( (  a )(

))

( (   )(

b a))

( (   )(

))

( (  d  )

(

B... Other (Non-Grid) Case Sections

The following sections store boundary conditions, material properties, and solver control settings.

B.... Zone

B.... Partitions

B.... Zone

or

Index:

xf-rp-tv

XF_RP_TV

C macro:

required

Status:

There is typically one zone section for each zone referenced by the grid. Although some grid zones

may not have corresponding zone sections, there cannot be more than one zone section for each

zone.

A zone section has the following form:

.

.

.

))

Grid generators and other preprocessors need only provide the section header and leave the list of

conditions empty, as in

.

.

.

))

on the zone type. When only zone-id, zone-type, zone-name, and domain-id are specified,

the index  is preferred for a zone section. However, the index  must be used if boundary condi-

tions are present, because any and all remaining information in a section of index  after zone-

id, zone-type, zone-name, and domain-id will be ignored.

Here the zone-id is in decimal format. This is in contrast to the use of hexadecimal in the grid sec-

tions.

axis

exhaust fan

fan

fluid

inlet vent

intake fan

interface

interior

mass-flow-outlet

outlet vent

outflow

periodic

radiator

shadow

solid

symmetry

wall

inside the domain. The interior type is used for the faces within a cell zone; the others are for

interior faces that form infinitely thin surfaces within the domain. ANSYS Fluent allows the wall type

to be assigned to face zones both on the inside and on the boundaries of the domain. Some zone

types are valid only for certain types of grid components. For example, cell (element) zones can be

assigned only one of the following types:

fluid

solid

All of the other types listed above can be used only for boundary (face) zones.

fluid

solid

The zone-name is a user-specified label for the zone. It must be a valid Scheme symbol  and is

written without quotes. The rules for a valid zone-name (Scheme symbol) are as follows:

The first character must be a lowercase letter  or a special-initial.

where a special-initial character is one of the following:

and a special-subsequent is one of the following:

. + -

Examples of valid zone names are inlet-port/cold!—, eggs/easy, and e=m*cˆ2.

Some examples of zone sections produced by grid generators and preprocessors are as follows:

The domain-id is an integer that appears after the zone name, associating the boundary condition

with a particular phase or mixture (sometimes referred to as phase-domains and mixture-domains).

Index:

xf-partition

XF_PARTITION

C macro:

only for partitioned grids

Status:

This section indicates each cell’s partition. The format of the section is as follows:

( (zone-id first-index last-index partition-count)(

p1

p2

p3

.

.

.

1See Revised () Report on the Algorithmic Language Scheme, William Clinger and Jonathan Rees (Editors),  November , Section

...

2The Standard actually only requires that case be insignificant; the ANSYS Fluent implementation accomplishes this by converting all

uppercase input to lowercase.

pn

))

where,

pn

))

where,

p1 = the partition of the cell whose ID is first-index

p2 = the partition of the cell whose ID is first-index

, and so on

pn = the partition of the cell whose ID is last-index

partition-count = the total number of partitions

Partition IDs must be between  and one less than partition-count.

B... Data Sections

The following sections store iterations, residuals, and data field values.

B.... Grid Size

B.... Data Field

B.... Residuals

Index:

xf-grid-size

XF_GRID_SIZE

C macro:

optional

Status:

This section indicates the number of cells, faces, and nodes in the grid that corresponds to the data

in the file. This information is used to check that the data and grid match. The format is

( (n-elements n-faces n-nodes))

where the integers are written in decimal.

Index:

xf-rf-seg-data

XF_RF_SEG_DATA

C macro:

required

Status:

This section lists a flow field solution variable for a cell or face zone. The data are stored in the same

order as the cells or faces in the case file. Separate sections are written out for each variable for each

face or cell zone on which the variable is stored. The format is

( (sub-section-id zone-id size n-time-levels

n-phases first-id last-id)

( data for cell or face with id = first-id

data-for-cell-or-face with id = first-id+

..

data-for-cell-or-face with id = last-id

))

where sub-section-id is a (decimal) integer that identifies the variable field (for example,  for

pressure,  for velocity). The complete list of these is available in the header file (xfile.h), which

is located in your installation area.

where,

where,

zone-id = the ID number of the cell or face

zone

size = the length of the variable vector

zone-id matches the ID used in case file. size is  for a scalar,  or  for a vector, equal to the

number of species for variables defined for each species). n-time-levels currently are not used.

A sample data file section for the velocity field in a cell zone for a steady-state, single-phase, 2D

problem is shown below:

( (      )

(.08462024e- .11823010e-

.78750622e- .15509699e-

.06139672e+ -.74040119e-

...

.33301604e+ -.04243895e-

.21703446e- -.46118382e-

.41687912e- -.27046436e-

.03528820e- -.01711005e-

))

The variables that are listed in the data file depend on the models active at the time the file is written.

Variables that are required by the solver based on the current model settings but are missing from

the data file are set to their default values when the data file is read. Any extra variables that are

present in the data file but are not relevant according to current model settings are ignored.

Index:

xf-rf-scaled-residuals

XF_RF_SCALED_RESIDUALS

C macro:

optional

Status:

This section lists the values of the residuals for a particular data field variable at each iteration:

( (n residual-section-id size domain-id)

(

iteration_number unscaled_residual scaling_factor

.

.

.

))

where,

n = the number of residuals

residual-section-id = an integer (decimal) indicating the

equation

domain-id = domain ID

where,

equation

size is  for a scalar,  or  for a vector, equal to the number of species for variables defined for

each species. The residual-section-id indicates the equation for which the residual is stored

in the section, according to the C constants defined in a header file (xfile.h) available in your in-

stallation area, as noted in Grid Sections (p. ).

The equations for which residuals are listed in the data file depend on the models active at the time

the file is written. If the residual history is missing from the data file for a currently active equation,

it is initialized with zeros.

This section describes the format of the ASCII text files that can be used as part of the setup for the

mesh morpher/optimizer, as described in Using the Mesh Morpher/Optimizer (p. ).

The following is an example of a file that can be read or written from the Define Control Points Dialog

Box (p. ):

Control Point Positions

CP No. X            Y             Z

. -. .

. . .

. . .

. . .

. . .

The following is an example of a file that can be read or written from the Motion Settings Dialog

Box (p. ) when Regular is selected from the Control Point Distribution list in the Regions tab of

the Mesh Morpher/Optimizer Dialog Box (p. ):

Reg     CP      Par      X       Y       Z

def-          par1     -

def-          par1            -

def-          par2

def-          par3

def-          par1

def-          par1            -

def-          par2

def-          par3

def-          par1

Box (p. ) when Unstructured is selected from the Control Point Distribution list in the Regions tab

of the Mesh Morpher/Optimizer Dialog Box (p. ):

Motion Definition

Name        Type        Par         Dir-x       Dir-y       Dir-z       Orig-x      Orig-y      Orig-z

rad-par1-  Rad         par-

tra-par2-  Trans       par-

rot-par3-  Rot         par-

Assignment to Control Points

Name        Control Points...

rad-par1-

When creating or editing a text file used to set up the mesh morpher/optimizer, note the following:

The file can be created from nothing using a text editor or spreadsheet program, as long as it adheres to

the formats described in this section. An easier alternative is to apply some sample definitions using the

appropriate dialog box, write a file, and then edit the file using a text editor or spreadsheet program.

The file must be a tab-delimited ASCII text file.

The names of the deformation regions (for example, def-), deformation parameters (for example, par1),

and motions (for example, tra-par2-) must correspond to those that exist in the intended case file.

When defining control points, the coordinates must lie within a deformation region in the intended case

file.

For the motion settings, the control point numbers must range between  and the maximum number of

available control points in the intended case file.

The direction components and coordinates can be any real numbers.

This section describes the format of the CSV files that can define shell conduction settings, as described

in Managing Shell Conduction Walls (p. ). The following is an example of such a file:

Zone ID,Zone Name,Layer Number,Material,Layer Thickness (m),Heat Generation Rate (w/m3)

,wall-,,substrate,.00E-,

,wall-,,gold,.50E-,

,wall-,,silicon,.00E-,.25E+

When creating or editing a file that defines the shell conduction settings, note the following:

the format described in this section. An easier alternative is to apply some sample shell conduction definitions

using the Shell Conduction Manager Dialog Box (p. ), generate a file using the Write... button, and then

edit the file using a text editor or spreadsheet program.

The file must be a comma-delimited ASCII file.

The first line contains the column headings shown in the previous example, and then each of the subsequent

lines define the settings for a layer.

The zone IDs, zone names, layer numbers, and materials (for example, wall-, substrate) must correspond

to those that exist in the intended case file.

The layer thicknesses must be positive, nonzero values.

Information will not be written for any wall that defines the heat generation rate using a UDF.

This section describes the format of the ASCII text files that can define the relationship between pressure

and flow rate for all of the 3D fan cell zones in a case file, as described in 3D Fan Zones (p. ). The

following is an example of such a file:

cell zone id

!CELL_ID

3D Fan Curve File Format

Pressure(Pa) Flowrate(m3/s)

. .

. .

. .

. .

. .

. .

. .

. .

. .

. .

!CELL_ID

. .

. .

. .

. .

. .

. .

. .

. .

. .

. .

. .

. .

When creating or editing a file that defines the 3D fan zone curve, note the following:

the format described in this section.

The file must be a tab-delimited ASCII file.

A single file can define multiple cell zones, but it must be read in each of the applicable Fluid dialog boxes.

For each section that defines the curve for a cell zone, the first three lines must follow the convention shown

in the previous example, and then each of the subsequent lines must list the experimental results.

The zone IDs (for example, ) must correspond to those that exist in the intended case file.

The units must match those in the case file.

Appendix C. Controlling CHEMKIN-CFD Solver Parameters Using

Text Commands

You have access to many parameter settings that can be used to control or improve the performance

and convergence behavior of the CHEMKIN-CFD solver within ANSYS Fluent. These parameters are ac-

cessed through the ANSYS Fluent Text User Interface (TUI), through typed text commands. This appendix

describes the available parameters, their default values, and their recommended use.

In general, default settings for the CHEMKIN-CFD parameters should be sufficient for most problems.

However, it may be necessary to change these settings to improve performance for specific types of

problems. In particular, the most appropriate solver parameters may vary depending on the nature of

the chemistry set.

For example, for chemistries with many trace species that have a large impact on solution results (that

is, the chemistry is “stiff”), solution tolerances should be relatively small (for example, .E- to .E-

for absolute tolerances and .E- to .E- for relative tolerances). For chemistry descriptions where all

of the species included are within a few orders of magnitude in terms of mass fraction, however, much

looser tolerances are more appropriate. Also, depending on the characteristic time scales of the dominant

chemical reactions, you may need to adjust the maximum time-step used by the CHEMKIN-CFD solver.

/define/models/species/CHEMKIN-CFD-parameters> basic-options

Print Level []

Absolute Tolerance For Gas Species [1e-]

Relative Tolerance For Gas Species [.]

Absolute Tolerance For Surface Species [1e-]

Relative Tolerance For Surface Species [.]

/define/models/species/CHEMKIN-CFD-parameters> advanced-options

Pseudo Time Stepping Solver Option (:Basic   :Robust) []

Pseudo Time Stepping Size [.]

Maximum Pseudo Time Step Attempts []

Maximum Time Step Allowed [.]

Minimum Time Step Allowed [1e-]

Initial Time Step For Solver []

Upper Bound For Gas Species Mass Fractions [.]

Lower Bound For Gas Species Mass Fractions [-1e-]

Upper Bound For Surface Species Mass Fractions [.]

Lower Bound For Surface Species Mass Fractions [-.]

Small Positive Value To Replace Negative Mass Fractions [1e-]

Enter Auxiliary Input Filename [""]

Enter Arbitrary String [""]

Enter Arbitrary Value []

Table : Summary of Basic CHEMKIN-CFD Parameters  (p. ) and Table : Summary of Advanced CHEMKIN-

CFD Parameters  (p. ) summarize basic and advanced parameters, respectively. These tables include

descriptions of the default values and physical units, where applicable, for each of the CHEMKIN-CFD

parameters, as well as a discussion of the recommended parameter usage.

Table : Summary of Basic CHEMKIN-CFD Parameters

Default

Value

Usage

Parameter

Controls the level of diagnostic printing to the

CHEMKIN-CFD diagnostic output file, where  indicates

Print Level

no printing,  indicates standard printing, and

enables a verbose level of printing that provides

details about the solver operations. Note that

diagnostic output can significantly contribute to

compute time such that high levels of printing should

be avoided unless problems are encountered that

require diagnosis.

.E-

Controls the smallest value of a species mass fraction

that will be tracked by the CHEMKIN-CFD solver

Absolute Toler-

ance for Gas-

phase Species

convergence algorithm. This should represent either

the smallest mass fraction that is of importance in

the problem or, for stiff chemistry, the smallest

fraction pertaining to a species that can have a

significant effect through chemical reaction on other

species of interest. Typical values range from .E- to

.E-.

.E-

Controls the accuracy to which gas species mass

fractions are resolved. Roughly this parameter controls

Relative Toler-

the number of significant digits in the solution.

However, this parameter can also be important for

convergence of problems with stiff chemistry, as it is

important to sufficiently resolve species that have a

major impact on trace species of interest. Typical

values range from .E- to .E-.

.E-

Controls the smallest value of a surface species site

fraction that will be tracked by the CHEMKIN-CFD

ance for Surface

Species

solver convergence algorithm. This should represent

either the smallest mass fraction that is of importance

in the problem or, for stiff chemistry, the smallest

.E-.

Controlling CHEMKIN-CFD Solver Parameters Using Text Commands

Default

Value

Usage

Parameter

.E-

Controls the accuracy to which surface species site

Species

Species

Table : Summary of Advanced CHEMKIN-CFD Parameters

Default

Value

Usage

Parameter

Determines which solver to use during pseudo

time-stepping used to improve the initial guess in a

Pseudo Time-step-

ping Solver Op-

tion

cell for steady-state simulations. By default, it is set

to  and a robust solver with strict error control will

be used when the steady-state algorithm requires

time-stepping assistance. You may optionally revert

to a less accurate time-stepping technique, which

may be computationally faster but more prone to

failure, by setting it to zero. See Advanced Parameters

Used in the Steady-State Solution Algorithm (p. )

for more information. This parameter is ignored for

transient simulations.

.E-

This option is only relevant if the Pseudo

Time-stepping Solver Option is set to  (the default

ping Size

[seconds]

setting). This controls the time interval for

time-stepping when time-stepping is used to assist

a steady-state calculation. See Advanced Parameters

for more information. A value of .E- seconds is

recommended for combustion problems.

This parameter controls how many iterations between

time-stepping and steady-state solution attempts can

Maximum Pseudo

Time-stepping At-

tempts

be tried before the solver gives up and registers a

failure for the cell. Usually only one attempt is needed,

but the maximum can be increased from this default

tempts

value in difficult cases. Note that in some cases it is

most efficient to ignore a small number of cell failures

early on in the simulation as long as these cells

recover on subsequent iterations. See Advanced

Parameters Used in the Steady-State Solution

Algorithm (p. ) for more information. A value of

to  is recommended to minimize error messages.

.E-

Maximum pseudo time-step value for time integration

during steady-state solution. This value is relevant to

steady-state simulations only.

Maximum Time

Step Allowed

[seconds]

Default

Value

Usage

Parameter

.E-

Minimum pseudo time-step value for time integration

Minimum Time

[seconds]

(i.e.,

not

specified)

Initial time-step value for use in time integration. By

default, the solver will automatically choose an

appropriate initial time step, which is the

Initial Time

Step for Solver

[seconds]

recommended approach. In rare cases, however,

control of initial time step value may improve

convergence behavior.

.

Sets the upper bounds for the gas-phase species mass

fractions during steady-state solution. In some cases,

Upper Bound for

Gas-species Mass

Fraction

it may help convergence to allow species to go

slightly over the physical bounds during interim

steady-state iterations rather than forcing the bounds

to be one.

.E-

Sets the lower bounds for the gas-phase species mass

Lower Bound for

Fraction

to be one.

.E-

Fraction

slightly negative during interim steady-state iterations

rather than forcing the bounds to be zero. A value as

negative as about -.E- may be used.

.

Sets the upper bounds for the surface species site

Surface Site

Fraction

to be one.

.E-

Sets the lower bounds for the surface species site

Fraction

rather than forcing the bounds to be zero.

.E-

This value will be used to substitute any non-positive

species fractions during interim steady-state iterations.

Small Positive

Value to Replace

In some cases, setting this to a very small positive

Negative Species

Fractions

number may aid convergence for the steady-state

solver.

““

Enter Auxiliary

Input Filename

““

Enter Arbitrary

String

Value

C.. Advanced Parameters Used in the Steady-State Solution Algorithm

Many of the parameters listed in Table : Summary of Advanced CHEMKIN-CFD Parameters  (p. ) are

relevant only for steady-state solution. Here a brief description of the steady-state solution algorithm

is provided in order to clarify the role of these parameters and their impact on solution convergence.

For steady-state problems, the ANSYS CHEMKIN-CFD solver is called by ANSYS Fluent for each cell during

each Fluent iteration towards a steady state. Within each cell, the chemistry solver will attempt to de-

termine an appropriate steady-state using a combination of a modified Newton-iteration procedure

and a “pseudo” time-stepping procedure. The Newton-iteration method is used to attempt to directly

iterate towards the desired solution. However, at early times in the simulation, this procedure may not

succeed, especially when the initial guess is far from the actual steady solution. In such cases, the

CHEMKIN-CFD module will automatically switch to a time-stepping mode to advance the initial guess

closer to the physical solution. After taking a certain number of time steps, the Newton-iteration algorithm

tries again. In this way, the steady-state solution is achieved with a minimum amount of time-stepping.

Since time-stepping is computationally expensive, this results in a computationally efficient but robust

method for achieving the steady-state solution.

You can control the number of times the CHEMKIN-CFD module is allowed to use time-stepping to

advance a solution towards steady-state before reporting a failure for any individual cell (see Maximum

Pseudo Time-stepping Attempts in Table : Summary of Advanced CHEMKIN-CFD Parameters

(p. )).

(p. )).

In performing the pseudo time-stepping procedure, there are two solver options - a “basic” time-stepping

procedure and a “robust” time-stepping procedure (see Pseudo Time-stepping Solver Option

in Table : Summary of Advanced CHEMKIN-CFD Parameters  (p. )). The “robust” procedure (default)

uses an integration method that is very accurate with error control enforced on all solution variables.

This can sometimes be more time consuming but is generally more reliable in tracking transient states

towards an eventual steady condition. The “basic” solver option is much more approximate in the time-

tracking technique, but is often faster and sufficiently robust for some cases.

When the “robust” time-stepping procedure is selected, you can specify the time interval used for each

attempt to advance the solution using time integration (See Pseudo Time-stepping Size in

Table : Summary of Advanced CHEMKIN-CFD Parameters  (p. )). The actual time steps used during

the time integration will be automatically determined based on the rate of change of the solution

variables. The time interval, however, controls the total time advanced before returning the solution to

be used as the next initial guess in the Newton-iteration.method.

In addition to the pseudo time-stepping controls, you may also control certain parameters that affect

the convergence behavior of the Newton-iteration algorithm itself. In particular, you can modify the

solution bounds imposed during the iterations (see Upper Bounds and Lower Bounds para-

meters in Table : Summary of Advanced CHEMKIN-CFD Parameters  (p. )). By extending the bounds

slightly outside of the physical limits, the Newton iteration can more easily resolve species fractions

that are very near to those limits. This can be especially helpful in early iterations where variable values

may be changing rapidly. It is also helpful to try to “reset” any negative species fractions to very small

values between iterations, so that these values do not have unphysical effects on reaction rates. For

this purpose, you can specify a small positive value, which should not exceed the specified absolute

tolerance, as a replacement value for negative fractions (see Small Positive Value to Replace

Negative Species Fractions in Table : Summary of Advanced CHEMKIN-CFD Parameters

(p. )).

Advanced Parameters Used in the Steady-State Solution Algorithm

C.. Setting Up Monitor Cells for the ANSYS CHEMKIN-CFD Chemistry

Solver

At the same level of the basic-options and advanced-options in the Text User Interface, that is, under

define/models/species/CHEMKIN-CFD-parameters, you can add, delete, and list monitor

cells.

By specifying a monitor cells in the CHEMKIN-CFD options, you are requesting additional printout

diagnostics for every iteration or time-step at this cell location. Such printout can add significantly to

computational times and should be avoided unless there is a problem has been encountered and more

diagnosis is needed.

Important

Using monitor cells may add significantly to the job run time. It is recommended that mon-

Important

itor cells only be included if extra diagnosis is required to resolve a convergence problem

or local mesh issue, for example.

Monitor cells are added using the add-cell-monitor option and providing the physical coordinates

that correspond as closely as possible to the centroid location of the desired cell in the Fluent mesh.

You can create more than one cell monitor and you can be delete all of them using the delete-cell-

monitor option. You may also list the currently activated monitor cells using the list-cell-

monitor option.

C.. Diagnostic Files and Error Messages

In addition to the standard ANSYS Fluent files produced during a run using the CHEMKIN-CFD solver,

the CHEMKIN-CFD module creates special files to hold diagnostic output and error messages that may

be helpful in diagnosing a problem with the pre-processing or run steps. In addition, error messages

may be written in the ANSYS Fluent Graphical User Interface window during run-time processing.

Table : Diagnostic Output Files Created During a CHEMKIN-CFD Run (p. ) lists additional files that

may be created by the chemistry solver, the data printed to them, and an indication of where they are

created in the ANSYS Fluent run process. All files are created within the working directory of the simu-

lation run. The actual names of many of the files will depend on variables, such as the chemistry-set

file names, the case-file name, the cell number, iteration or time-step number, and the processor id.

Such variables are indicated by < > in Table : Diagnostic Output Files Created During a CHEMKIN-CFD

Run (p. ).

Table : Diagnostic Output Files Created During a CHEMKIN-CFD Run

Run (p. ).

Contents Description

When File Is Created

Filename

This file echoes back the gas-phase

chemistry reaction set, species names, and

Always created during

pre-processing, upon

<gas_chem-

istry>.out

elements in formatted text. In addition,

saving the CHEMKIN

mechanism definition.

detailed error messages are contained in

this file in case an error is encountered

while processing the gas-phase chemistry

input file and gas-phase thermodynamic

data.

Filename

A “Linking File” used to transfer the

pre-processed information to the

chem.asc

CHEMKIN-CFD module at run-time. This file

is typically not viewed by the user, but may

occasionally be requested by Technical

Support during problem diagnosis.

This file echoes back the surface chemistry

reaction set and the surface phase and

Created during

pre-processing, only if

<surface_chem-

species names. In addition, detailed error

surface chemistry box

messages are contained in this file in case

is checked in CHEMKIN

an error is encountered while processing

the surface chemistry input file and

surface-species thermodynamic data.

surf.asc

surf.asc

This file echoes back the transport-data

fitting coefficients in formatted text. In

<trans-

port_data>.out

addition, detailed error messages are

transport-property box

contained in this file in case an error is

encountered while processing the

gas-phase transport data.

tran.asc

occasionally be requested by ANSYS

Technical Support during problem

diagnosis.

Messages are written to this file that record

the progress of chemistry-set pre-processor

Created when the

simulation run is

KINetics-

log.txt

and CHEMKIN-CFD solver. The printing level

initiated in the

during the simulation run can be controlled

subdirectory flu-

entKINlog.

by Print Level as indicated in

Table : Summary of Basic CHEMKIN-CFD

Parameters  (p. ).

Includes debug information, including the

actual input sent into the CHEMKIN-CFD

Created for Monitor

Cells (see Setting Up

KIN-

CELL_<cell_id>_<it-

module by ANSYS Fluent for the particular

Monitor Cells for the

eration_num-

ber>.DBG

cell and iteration. This information may be

requested by ANSYS Technical Support

when diagnosing cell failures.

ANSYS CHEMKIN-CFD

Chemistry

ber>.DBG

Chemistry

Solver (p. )) at every

iteration or time-step,

any time that the

(Table : Summary of

Diagnostic Files and Error Messages

Filename

Basic CHEMKIN-CFD

Parameters  (p. )) is

>. Also created any

time that a cell fails in

the CHEMKIN-CFD

solver and the Print

Level is >.

C.. Error Messages Printed in the ANSYS Fluent Graphical User Interface

Advanced Parameters Used in the Steady-State Solution Algorithm (p. ) lists possible error messages

that may appear in the ANSYS Fluent Graphical User Interface during run using the CHEMKIN-CFD

solver. The table includes recommended actions that may help resolve or narrow down the problem.

In some cases, you may be referred to some of the additional diagnostic output files generated by the

CHEMKIN-CFD module and listed in Table : Diagnostic Output Files Created During a CHEMKIN-CFD

Run (p. ).

Table : Error Messages that May Be Printed to the Fluent GUI

Value

Setting

Verify the filename and file path for the

gas-phase chemistry input file in the Import

Cannot read gas-phase chemistry

input file.

CHEMKIN Format Mechanism dialog box and

re-import.

Verify the filename and file path for the surface

chemistry input file in the Import CHEMKIN

Format Mechanism dialog box and re-import.

Cannot read surface chemistry

thermodynamic data file in the Import

Cannot read thermodynamic data

file.

file.

transport-property data file in the Import

Cannot read transport properties

data file.

Check the <gas_chemistry>.out file in

the working directory for error messages.

linking data file during gas-

phase pre-processing.

linking data file during surface

pre-processing.

linking data file during trans-

port pre-processing.

Check the <surface_chemistry>.out file

in the working directory for error messages.

Value

Setting

Check the <transport_data>.out file in

Check file permissions on working directory

and make sure that there is only one

Cannot write gas-phase chemistry

output file.

CHEMKIN-CFD process using these files at a

time.

Cannot write surface chemistry

time.

Cannot write transport properties

time.

time.

time.

linking data file.

time.

time.

time.

Verify gas-phase chemistry file path in the

CHEMKIN Mechanism definition and re-import

the chemistry files.

Gas-phase chemistry file is NULL.

Verify surface-chemistry file path in the

Surface chemistry file is NULL.

Verify thermodynamic-data file path in the

the chemistry files

Thermodynamic data file is NULL.

Verify transport-data file path in the CHEMKIN

Mechanism definition and re-import the

chemistry files.

Transport properties data file

is NULL.

Failure in pre-processing of gas-

phase chemistry mechanism.

Failure in pre-processing of

surface chemistry mechanism.

transport properties.

Error Messages Printed in the ANSYS Fluent Graphical User Interface

Value

Setting

Check to see if the ANSYS Fluent solution has

diverged or has unphysical values for the

Failure in CHEMKIN Gas-phase

library call.

variables. Try turning Print Level >  and

setting a monitor cell to obtain more

Failure in CHEMKIN Surface lib-

rary call.

Failure in CHEMKIN Transport

Re-import the CHEMKIN chemistry set and

make sure it is selected in the Species Model

dialog box (under Setup/Models).

Need to run CHEMKIN-CFD PrePro-

cess first.

Either de-select the Surface Chemistry option

in the Import CHEMKIN Format Mechanism

No surface data for the chemistry

set.

dialog box, or make sure that a valid surface

chemistry file is indicated.

Either de-select the Transport Data option in

the Import CHEMKIN Format Mechanism

No transport data for the chem-

istry set.

dialog box, or make sure that a valid transport

data file is indicated.

Check file permissions on the working directory

Failure in writing data into the

diagnostics file.

time.

Check the KINetics-log.txt file in the

time.

subdirectory fluentKINlog for error

Error in CHEMKIN-CFD model, see

diagnostic output file for de-

tails.

messages. See Error Messages Printed in the

ANSYS Fluent Graphical User Interface (p. )

C.. Diagnostic Messages in the KINetics-log.txt File

The KINetics-log.txt file is a “catch-all” for many diagnostic messages that are generated by the

CHEMKIN-CFD module. The most common types of messages are error messages related to setup or

cell convergence.

Cell-convergence error messages can take a variety of forms. The most common are summarized in

Table : Other Error Messages in KINetics-log.txt (p. ). In general, if there are just a few failed

cells at the beginning of a simulation it is safe to ignore them. When the number of failed cells continues

to grow with each iteration, there is likely an issue with the problem set-up or with the chemistry data.

Table : Other Error Messages in KINetics-log.txt (p. ) contains some broad suggestions of

ways to improve cell-convergence behavior based on the type of cell failure message received.

Table : Other Error Messages in KINetics-log.txt

Recommended Action

Error Message

Most likely suggests an error in setting the

convergence criteria (that is absolute and

FAILURE INITIALIZING SETTINGS FOR

THE KINetics STEADY-STATE GAS-

PHASE CHEMISTRY SOLVER

relative tolerance) and the pseudo-steady-state

time stepping parameters. Check that the

user-provided values are reasonable.

Indicates that a convergence problem was

encountered during steady-state solution,

WARNING: Exceeded allowed time-

stepping intervals in cell

where time-stepping is used to help advance

the steady-state iterations. In this case, you can

either ignore the message (see if the cell

convergence recovers in subsequent iterations)

or try to increase either the time interval or

the number of allowed time-stepping intervals

(See Table : Summary of Advanced

CHEMKIN-CFD Parameters  (p. ) for more

information).

Indicates that the cell failed to converge (either

steady-state or transient).In this case, you can

KINETICS ERROR: SOLUTION FAILED

or try to modify some of the user-controlled

parameters to improve convergence (See

Table : Summary of Advanced CHEMKIN-CFD

Parameters  (p. ) for more information).

Indicates that the problem is difficult to

converge so that the transient solver is taking

Warning - The transient chemistry

solver tried  steps without

extra steps. However, it is only a warning and

convergence in this cell;

more steps will be allowed

the cell has not actually failed. If you receive

an excessive number of these messages, try

reducing the absolute or relative solution

tolerances that control the CHEMKIN-CFD

solver.

Indicates a possible error in the pre-processing

of the gas-phase chemistry input file. Check

KINETICS ERROR: Problem getting

species names; Check that the

the <gas_chemistry>.out file for error

messages.

CHEMKIN files have been processed

correctly

messages.

correctly

of the surface chemistry input file. Check the

surface chemistry info; Check

<surface_chemistry>.out file for error

messages.

that the CHEMKIN files have been

processed correctly

These messages are from the CHEMKIN-CFD

transient solver, DASPK. The exact message

DASPK:...

Diagnostic Messages in the KINetics-log.txt File

usually contains more information about the

problem.

Note

During steady-state simulations, once an iteration occurs where there are no failed cells, the

effect of previously failed cells in earlier iterations is completely erased.

Appendix D. Nomenclature

Area (m2, ft2)

Acceleration (m/s2, ft/s2)

Local speed of sound (m/s, ft/s)

Concentration (mass/volume, moles/volume)

Drag coefficient, defined different ways (dimensionless)

Heat capacity at constant pressure, volume (J/kg-K, Btu/lbm- °F)

,

Diameter; dpDp, particle diameter (m, ft)

Hydraulic diameter (m, ft)

Mass diffusion coefficient (m2/s, ft2/s)

Total energy, activation energy (J, kJ, cal, Btu)

Mixture fraction (dimensionless)

Force vector (N, lbf)

Drag force (N, lbf)

Gravitational acceleration (m/s2, ft/s2); standard values = . m/s2, . ft/s2

Grashof number

ratio of buoyancy forces to viscous forces (dimensionless)

Gr

Total enthalpy (energy/mass, energy/mole)

Heat transfer coefficient (W/m2-K, Btu/ft2-h- °F)

Species enthalpy; h0, standard state enthalpy of formation (energy/mass, energy/mole)

Gr

Radiation intensity (energy per area of emitting surface per unit solid angle)

Mass flux; diffusion flux (kg/m -s, lbm/ft2-s)

Equilibrium constant = forward rate constant/backward rate constant (units vary)

Kinetic energy per unit mass (J/kg, Btu/lb m)

Reaction rate constant, for example,

,

,

,

(units vary)

Thermal conductivity (W/m-K, Btu/ft-h- °F)

Boltzmann constant (

J/molecule-K)

Mass transfer coefficient (units vary); also

,

,

Length scale (m, cm, ft, in)

Lewis number

ratio of thermal diffusivity to mass diffusivity (dimensionless)

Le

Mass (g, kg, lbm)

Mass flow rate (kg/s, lbms)

Molecular weight (kg/kmol, lbm/lbmmol)

ratio of fluid velocity magnitude to local speed of sound (dimensionless)

M

dimensionless heat transfer or mass transfer coefficient (dimensionless);

usually a function of other dimensionless groups

Nu

Pressure (Pa, atm, mm Hg, lbf/ft2)

Peclet number

for heat transfer, and

for mass transfer (dimensionless)

Pe

Prandtl number

ratio of momentum diffusivity to thermal diffusivity (dimensionless)

Pr

Flow rate of enthalpy (W, Btu/h)

Heat flux (W/m2, Btu/ft2-h)

Gas-law constant (.

J/kmol-K, . Btu/lbmmol- °F)

Radius (m, ft)

Reaction rate (units vary)

Rayleigh number

; measure of the strength of buoyancy-induced flow in natural (free)

convection (dimensionless)

Ra

ratio of inertial forces to viscous forces (dimensionless)

Re

Total entropy (J/K, J/kmol-K, Btu/lbmmol- °F)

Species entropy; s0, standard state entropy (J/kmol-K, Btu/lbmmol- °F)

Schmidt number

Re

ratio of momentum diffusivity to mass diffusivity (dimensionless)

Sc

Mean rate-of-strain tensor (s-)

Temperature (K, °C, °R, °F)

Time (s)

Free-stream velocity (m/s, ft/s)

Velocity magnitude (m/s, ft/s); also written with directional subscripts (for example, vx, vy, vz,

vr)

Volume (m3, ft3)

Overall velocity vector (m/s, ft/s)

Weber number

ratio of aerodynamic forces to surface tension forces (dimensionless)

We

Mole fraction (dimensionless)

Mass fraction (dimensionless)

Permeability, or flux per unit pressure difference (L/m2-h-atm, ft /ft2-h-(lbf/ft2))

Thermal diffusivity (m2/s, ft2/s)

Volume fraction (dimensionless)

Coefficient of thermal expansion (K

)

Porosity (dimensionless)

Ratio of specific heats, cp/cv (dimensionless)

Change in variable, final

initial (for example, Δp, Δt, ΔH, ΔS, ΔT)

Nomenclature

Delta function (units vary)

Emissivity (dimensionless)

Lennard-Jones energy parameter (J/molecule)

Turbulent dissipation rate (m2/s3, ft2/s3)

Void fraction (dimensionless)

Effectiveness factor (dimensionless)

Rate exponents for reactants, products (dimensionless)

,

Radiation temperature (K)

Molecular mean free path (m, nm, ft)

Wavelength (m, nm, Å, ft)

Dynamic viscosity (cP, Pa-s, lbm/ft-s)

Kinematic viscosity (m2/s, ft2/s)

Stoichiometric coefficients for reactants, products (dimensionless)

,

Density (kg/m3, lbm/ft3)

Stefan-Boltzmann constant (.67x10- W/m2-K4)

Surface tension (kg/m, dyn/cm, lbf/ft)

Scattering coefficient (m-)

Stress tensor (Pa, lbf/ft2)

Shear stress (Pa, lbf/ft2)

Time scale, for example,

,

,

(s)

,

,

(s)

Tortuosity, characteristic of pore structure (dimensionless)

Equivalence ratio (dimensionless)

Thiele modulus (dimensionless)

Angular velocity;

, Mean rate of rotation tensor (s-)

Specific dissipation rate (s-)

Solid angle (degrees, radians, gradians)

Diffusion collision integral (dimensionless)

Important

[] CRANIUM, Version .. Molecular Knowledge Systems, Inc., Bedford, NH. .

[] FIELDVIEW Reference Manual, Software Release Version . Intelligent Light. .

[] KINetics for Fluent, Version .. Reaction Design, Inc., San Diego, CA. .

[] VdmTools Programmer Manual, Version ... Visual Kinematics, Inc. .

[] T. Ahmad, S. L. Plee, and J. P. Myers. "Computation of Nitric Oxide and Soot Emissions from Turbulent

Diffusion Flames". J. of Engineering for Gas Turbines and Power. . –. .

[] A. A. Amsden, P. J. O’Rourke, and T. D. Butler. "KIVA-: A Computer Program for Chemically Reactive

Flows with Sprays". Technical Report LA--MS, UC-. Los Alamos National Laboratory, Los

Alamos, New Mexico. May .

[] M. J. Assael, J. P. M. Trusler, and T. F. Tsolakis. "Thermophysical Properties of Fluids". Technical report.

Imperial College Press, London. .

[] R. H. Aungier. "A Fast, Accurate Real Gas Equation of State for Fluid Dynamic Analysis Applications".

Journal of Fluids Engineering. . –. .

[] R. Barrett, M. Berry, T. F. Chan, J. Demmel, J. Donato, J. Dongarra, V. Eijkhout, R. Pozo, C. Romine,

and H. Van der Vorst. "Templates for the Solution of Linear Systems: Building Blocks for Iterative

Methods". SIAM, 2nd edition. Philadelphia, Pennsylvania. .

[] A. Bejan. Convection Heat Transfer. John Wiley and Sons, New York. .

[] D. T. Blackstock. Fundamentals of Physical Acoustics. John Wiley & Sons. .

[] C. T. Bowman. "Chemistry of Gaseous Pollutant Formation and Destruction”. Fossil Fuel Combustion.

W. Bartok and A. F. Sarofim, editors. J. Wiley and Sons, Canada. .

[] R. N. Bracewell. The Fourier transform and its applications. McGraw Hill. .

[] W. Brack, B. Heine, F. Birkhold, M. Kruse, O. Deutschmann. "Formation of Urea-Based Deposits in an

Exhaust System: Numerical Predictions and Experimental Observations on a Hot Gas Test Bench".

Emiss. Control Sci. Technol.. . . –. .

[] W.-P. Breugem. “The Effective Viscosity of a Channel-type Porous Medium”. Phys. of Fluids. . . .

[] H. Brinkman. “A Calculation of the Viscous Force Exerted by a Flowing Fluid on a Dense Swarm of

Particles”. Applied Scientific Research. A1. –.

[] H. Brinkman. “The Viscosity of Concentrated Suspensions and Solutions”. J. Chem. Phys. . . –.

.

[] R. J. Brooks and A. T. Corey. “Hydraulic properties of porous media”. Hydrology Paper . Colorado State

University. Fort Collins, Colorado, USA. .

[] S. J. Brookes and J. B. Moss. "Prediction of Soot and Thermal Radiation in Confined Turbulent Jet Diffusion

Flames". Combustion and Flame. . –. .

[] R. Carsel and R. Parrish. “Developing joint probability distributions of soil water retention characteristics”.

Water Resources Research. . . –. .

[] J. R. Cash and A. H. Karp. "A variable order Runge-Kutta method for initial value problems with rapidly

varying right-hand sides". ACM Transactions on Mathematical Software. . –. .

[] T. Cebeci and P. Bradshaw. Momentum Transfer in Boundary Layers. Hemisphere Publishing Corpor-

ation, New York. .

[] P. J. Coelho and M. G. Carvalho. "Modeling of Soot Formation and Oxidation in Turbulent Diffusion

Flames". J. of Thermophysics and Heat Transfer. (). –. .

[] M. F. Cohen and D. P. Greenberg. "The Hemi-Cube: A Radiosity Solution for Complex Environments".

Computer Graphics. (). –. .

[] H. W. Coleman, B. K. Hodge, and R. P. Taylor. "A Re-Evaluation of Schlichting’s Surface Roughness Ex-

periment". Journal of Fluids Engineering. . .

[] E. H. Cuthill and J. McKee. "Reducing Bandwidth of Sparse Symmetric Matrices". In Proc. ACM 24th

National Conf. New York. –. .

[] J. F. Daunenhofer and J. R. Baron. "Grid Adaption for the 2D Euler Equations". Technical Report AIAA-

. American Institute of Aeronautics and Astronautics. .

[] J. E. Dec. "A Conceptual Model of DI Diesel Combustion Based on Laser Sheet Imaging". SAE Technical

Paper . SAE. .

[] J. Ding and D. Gidaspow. "A Bubbling Fluidization Model Using Kinetic Theory of Granular Flow". AIChE

J. (). –. .

[] Y. Egorov and F. Menter. "Experimental Implementation of the RPI Wall Boiling Model in CFX-. ".

Technical Report. ANSYS/TR--, ANSYS GmbH. .

J. (). –. .

[] S. Ergun. "Fluid Flow through Packed Columns". Chem. Eng. Prog. (). –. .

[] G. M. Faeth. "Spray Atomization and Combustion". Technical Report -. AIAA. .

[] J. E. Ffowcs-Williams and D. L. Hawkings. "Sound Generation by Turbulence and Surfaces in Arbitrary

Motion". Proc. Roy. Soc. London. A264. –. .

[] E. U. Finlayson, D. K. Arasteh, C. Huizenga, M. D. Rubin, and M. S. Reilly. "WINDOW . : Documentation

of Calculation Procedures". Technical Report Publication LBL-/ TA-. Lawrence Berkeley

Laboratory, Energy and Environmental Division, Berkeley, CA . .

[] K.–Y. Fung and H. Ju. "Broadband Time-Domain Impedance Models”. AIAA Journal. (). January

.

[] K.–Y. Fung, H. Ju, and B. Tallapragada. "Impedance and Its Time-Domain Extensions”. AIAA Journal.

(). –. January .

[] M. T. van Genuchten. “A closed form equation for predicting the hydraulic conductivity of unsaturated

soils”. Soil Science Society of American Journal. . . –. .

[] T. Gessner. "Dynamic Mesh Adaption for Supersonic Combustion Waves Modeled with Detailed Reaction

Mechanisms". PhD thesis. University of Freiburg, Freiburg, Germany. .

[] A. Ghobadian and S. A. Vasquez. "A General Purpose Implicit Coupled Algorithm for the Solution of

Eulerian Multiphase Transport Equation". International Conference on Multiphase Flow. Leipzig,

Germany. .

[] N. E. Gibbs, W. G. Poole, Jr., and P. K. Stockmeyer. "An algorithm for reducing the bandwidth and

profile of a sparse matrix". SIAM J. Numer. Anal. . –. .

[] M. B. Giles. "Non-Reflecting Boundary Conditions for the Euler Equations". Technical Report -.

Computational Fluid Dynamics Laboratory, Massachusetts Institute of Technology, Cambridge,

MA. .

[] R.A. Gore and C.T. Crowe. “Effect of particle size on modulating turbulent intensity”. Int. J. Multiphase

Flow. . –. .

[] J. Gottgens, F. Mauss, and N. Peters. "Analytic Approximations of Burning Velocities and Flame Thick-

nesses of Lean Hydrogen, Methane, Ethylene, Ethane, Acetylene and Propane Flames". In Twenty-

Fourth Symposium (Int.) on Combustion, Pittsburgh. –. .

[] P. M. Gresho, R. L. Lee, and R. L. Sani. "On the Time-Dependent Solution of the Incompressible Navier-

Stokes Equations in Two and Three Dimensions". In Recent Advances in Numerical Methods in Fluids.

Pineridge Press, Swansea, U. K. .

[] R. J. Hall, M. D. Smooke, and M. B. Colket. Physical and Chemical Aspects of Combustion. Gordon and

Breach. .

[] R. A. W. M. Henkes and C. J. Hoogendoorn. "Scaling of the Turbulent Natural Convection Flow in a

Heated Square Cavity". Trans. of the ASME. . –. May .

[] J. B. Heywood. Internal Combustion Engine Fundamentals. McGraw-Hill, New York, rev. edition. .

[] C. Hirsch. Numerical Computation of Internal and External Flows: Computational Methods for Inviscid

and Viscous Flows, volume . John Wiley & Sons, New York. .

[] J. O. Hirschfelder, C. F. Curtiss, and R. B. Bird. Molecular Theory of Gases and Liquids. John Wiley &

Sons, New York. .

[] K. Hsu and A. Jemcov. "Numerical investigation of detonation in premixed hydrogen-air mixture - as-

sessment of simplified chemical mechanisms". Technical Report AIAA--. American Institute

of Aeronautics and Astronautics, Fluids  Conference and Exhibit, Denver, CO. June .

[] Y. Y. Hsu. "On the size range of active nucleation cavities on a heating surface". J. Heat Transfer. ().

–. August .

[] G. W. Jackson and D. F. James. "The Permeability of Fibrous Porous Media". Canadian Journal of

Chemical Engineering. (). –. June .

[] A. Jemcov and J. P. Maruszewski. "Shape Optimization Based on Downhill Simplex Optimizer and Free-

Form Deformation in General Purpose CFD Code". 17th Annual Conference of CFD Society of Canada.

Ottawa, Ontario, Canada. .

[] P. C. Johnson and R. Jackson. "Frictional-Collisional Constitutive Relations for Granular Materials, with

Application to Plane Shearing". J. Fluid Mech. . –. .

[] G. Karypis and V. Kumar. METIS - A Software Package for Partitioning Unstructured Graphs, Partitioning

Meshes, and Computing Fill-Reducing Orderings of Sparse Matrices, Version .. Manual. University

of Minnesota and Army HPC Research Center. .

[] G. Karypis and K. Schloegel. PARMETIS - Parallel Graph Partitioning and Sparse Matrix Ordering Library,

Version .. Manual. University of Minnesota. .

[] A. Kaufmann, F. Nicoud, and T. Poinsot. Flow Forcing Techniques for Numerical Simulation of Combustion

Instabilities. Combustion and Flame. . –. .

[] R. J. Kee, F. M. Rupley, and J. A. Miller. "SURFACE CHEMKIN: A Software Package for the Analysis of

Heterogeneous Chemical Kinetics at a Solid-Surface - Gas-Phase Interface". Technical Report SAND

. Sandia National Labs. .

[] R. J. Kee, F. M. Rupley, J. A. Miller, M. E. Coltrin, J. F. Grcar, E. Meeks, H. K. Moffat, A. E. Lutz, G. Dixon-

Lewis, M. D. Smooke, J. Warnatz, G. H. Evans, R. S. Larson, R. E. Mitchell, L. R. Petzold, W. C.

Reynolds, M. Caracotsios, W. E. Stewart, P. Glarborg, C. Wang, O. Adigun, W. G. Houf, C. P. Chou,

S. F. Miller, P. Ho, and D. J. Young. CHEMKIN v. .. Technical Report. San Diego, CA. Reaction

Design, Inc. .

[] T. G. Kolda, R. M. Lewis, and V. Torczon. "Optimization by Direct Search: New Perspectives on Some

Classical and Modern Methods". SIAM Review. . . –. .

[] B. Koncar, I. Kljenak, and R. Mavko. "Modeling of Local Two-Phase Flow Parameters in Upward Subcooled

Flow Boiling at Low Pressure". International Journal of Heat and Mass Transfer. . –.

.

[] K. K. Y. Kuo. Principles of Combustion. John Wiley and Sons, New York. .

[] B. E. Launder and D. B. Spalding. "The Numerical Computation of Turbulent Flow". Computer Methods

in Applied Mechanics and Engineering. . –. .

[] M. C. Leverett. “Capillary behavior in porous solids”. Transactions of the AIME. . –. .

[] J. Li, Z. Zhao, et al. "On Sound Generated Aerodynamically". Proc. Roy. Soc. London. A211. –.

.

[] M. J. Lighthill. "A Comprehensive Kinetic Mechanism for CO, CH2O, and CH3OH Combustion". Int. J.

Chem. Kinet. . -. .

[] P. Lin. Numerical Modeling of Water Waves. Taylor & Francis. .

[] R. P. Lindsted, F. C. Lockwood, and M. A. Selim. "Rate Constants Based on Partial Equilibrium Assump-

tions". Internal Report No. TF//, Technical report. Imperial College, London, UK. .

[] M. S. Liou. "A sequel to AUSM: AUSM+". Journal of Computational Physics. . –. .

[] F. C. Lockwood, S. M. A. Rizvi, and N. G. Shah. "Comparative Predictive Experience of Coal Firing". In

Proceedings Inst. Mechanical Engineers. . –. .

[] J. Y. Luo, R. I. Issa, and A. D. Gosman. "Prediction of Impeller-Induced Flows in Mixing Vessels Using

Multiple Frames of Reference". In I ChemE Symposium Series. . –. .

[] B. F. Magnussen and B. H. Hjertager. "On mathematical models of turbulent combustion with special

emphasis on soot formation and combustion". In 16th Symp. (Int’l.) on Combustion. The Combustion

Institute. .

[] M. Manninen, V. Taivassalo, and S. Kallio. "On the mixture model for multiphase flow". VTT Publications

. Technical Research Centre of Finland. .

[] B. J. McBride, S. Gordon, and M. A. Reno. "Coefficients for Calculating Thermodynamic and Transport

Properties of Individual Species". NASA TM-. October .

[] H. A. McGee. Molecular Engineering. McGraw-Hill, New York. .

[] K. I. M. McKinnon. "Convergence of the Nelder-Mead Simplex Method a Nonstationary Point ". SIAM J.

Optimization. . . –. .

[] F. R. Menter and Y. Egorov. "Re-visiting the Turbulent Scale Equation". Proc. IUTAM Symp. One Hundred

Years of Boundary Layer Research, Göttingen. Springer. .

[] F. R. Menter and Y. Egorov. "A Scale-Adaptive Simulation Model Using Two-Equation Models". AIAA

Paper--. Reno NV. .

[] H. J. Merk. "The Macroscopic Equations for Simultaneous Heat and Mass Transfer in Isotropic, Continuous

and Closed Systems". Appl. Sci. Res. . –. .

[] R. Merz, J. Kruckels, J. Mayer, and H. Stetter. "Computation of Three Dimensional Viscous Transonic

Turbine Stage Flow Including Tip Clearance Effects". ASME -GT-. .

[] C. V. Naik, K. V. Puduppakkam, et al. "Modeling Combustion Characteristics of Components of Model-

Biodiesel at High Temperatures". WSS/CI Spring  Meeting. Los Angeles, CA. .

[] J. A. Nelder and R. Mead. "A Simplex Method for Function Minimization". Computer Journal. . .

–. .

[] Y.I. Oka et al.. "Practical estimation of erosion damage caused by solid particle impact, Part : Effects

of impact parameters on a predictive equation". 15th International Conference on Wear of Materials.

. -. –. .

[] P. J. O’Rourke. "Collective Drop Effects on Vaporizing Liquid Sprays". PhD thesis. Princeton University,

Princeton, New Jersey. .

[] M. Østberg, P. Glarborg, A. Jensen, J. E. Johnsson, L. S. Pedersen, and K. Dam-Johansen. "A model

of the coal reburning process". In Proc. Combust Inst. . –. .

[] I. Owczarek and K. Blazej. "Recommended Critical Temperatures. Part I. Aliphatic Hydrocarbons". J.

Phys. Chem. . –. .

[] I. Owczarek and K. Blazej. "Recommended Critical Pressures. Part I. Aliphatic Hydrocarbons". J. Phys.

Chem. . –. .

[] S. V. Patankar. Numerical Heat Transfer and Fluid Flow. Hemisphere, Washington, DC. .

[] S. V. Patankar, C. H. Liu, and E. M. Sparrow. "Fully Developed Flow and Heat Transfer in Ducts Having

Streamwise-Periodic Variations of Cross-Sectional Area". ASME J. of Heat Transfer. . –.

.

[] D. Y. Peng and D. B. Robinson. "A New Two-Constant Equation of State". Industrial and Engineering

Chemistry: Fundamentals. . –. .

[] R. H. Perry, D. W. Gree, and J. O. Maloney. Perry’s Chemical Engineers’ Handbook. McGraw-Hill, New

York, 6th edition. .

[] A. A. F. Peters and R. Weber. "Mathematical Modeling of a . MWt Swirling Natural Gas Flame. Part

: Eddy Break-up Concept for Turbulent Combustion; Probability Density Function Approach for Nitric

Oxide Formation". Combustion Science and Technology. . –. .

[] T. J. Poinsot and S. K. Lele. "Boundary Conditions for Direct Simulation of Compressible Viscous Flows".

Journal of Computational Physics. . –. .

[] T. J. Poinsot and L. Selle. "Actual Impedance of Nonreflecting Boundary Conditions: Implications for

Computation of Resonators". AIAA Journal. (). –. May .

[] B. E. Poling, J. M. Prausnitz, and J. P. O’Connell. The properties of Gases and Liquids. McGraw-Hill, In-

ternational Edition, 5th edition. .

[] S. B. Pope. ISAT-CK (Version .) User’s Guide and Reference Manual. .

[] M. J. D. Powell. "The NEWUOA software for unconstrained optimization without derivatives". Large-

Scale Nonlinear Optimization (Nonconvex Optimization and Its Applications). . –. G. Di

Pillo and M. Roma, editors. Springer. .

[] W. H. Press, S. A. Teukolsky, W. T. Vetterling, and B. P. Flannery. Numerical Recipes: The Art of Scientific

Computing, Third Edition. Cambridge University Press, Cambridge, England. .

[] C. L. Rasmussen and A. E. Rasmussen. "Sensitizing Effects of NOx on CH4 Oxidation at High Pressure".

Comb. Flame. . . .

[] O. Redlich and J. N. S. Kwong. "On the Thermodynamics of Solutions. An Equation of State. Fugacities

of Gaseous Solutions". Chem. Rev. . . -. .

[] W. C. Reynolds. Thermodynamic Properties in SI: Graphs, Tables, and Computational Equations for

Substances. Department of Mechanical Engineering, Stanford University. .

[] J. W. Rose and J. R. Cooper. Technical Data on Fuel. Scottish Academic Press, Edinburgh. .

[] J. W. Rose and J. R. Cooper, editors. Technical Data on Fuels. Wiley, 7th edition. .

[] H. H. Rosenbrock. "An Automatic Method for Finding the Greatest or Least Value of a Function".

Computer Journal. . . –. .

[] F. Qian, L. Lu, T.Feng, and D.Yang. "Experimental and 3D Embedded Modelling for Diesel Engine SCR

Deposit". International Journal of Automotive Technology. . . –. .

[] Y. Saad and M. H. Schultz. "GMRES: A Generalized Minimal Residual Algorithm for Solving Nonsym-

metric Linear Systems". SIAM J. Sci. and Stat. Comput. (). –. July .

[] A. Saxer. "A Numerical Analysis of a 3D Inviscid Stator/Rotor Interaction Using Non-Reflecting Boundary

Conditions". PhD thesis. Massachusetts Institute of Technology, Cambridge, Massachusetts. March

.

[] S. Sarkar and L. Balakrishnan. "Application of a Reynolds-Stress Turbulence Model to the Compressible

Shear Layer". ICASE Report -18NASA CR . .

[] P. R. Spalart, S. Deck, M. L. Shur, K. D. Squires, M. Kh. Strelets, and A. Travin. "A New Version of De-

tached-eddy Simulation, Resistant to Ambiguous Grid Densities ". Theoretical and Computational

Fluid Dynamics. Springer Berlin / Heidelberg. Volume , Number . July, .

[] H. Schlichting. Boundary-Layer Theory. McGraw-Hill, New York. .

[] H. Schlichting and K. Gersten. Grenzschicht-Theorie. Springer-Verlag, Berlin, Heidelberg, New York.

.

[] A. A. Shabana. Computational Dynamics. John Wiley and Sons, New York. .

.

[] J. Shin and T. H. Bond. "Experimental and Computational Ice Shapes and Resulting Drag Increase for

a NACA  Airfoil". NASA Technical Memorandum . .

[] G. M. Shroff and H. B. Keller. "Stabilization of unstable procedures: The recursive projection method".

SIAM J. Numer. Anal. (). –. .

[] M. L. Shur, P. R. Spalart, M. K. Strelets, and A. K. Travin. "A Hybrid RANS-LES Approach With Delayed-

DES and Wall-Modelled LES Capabilities". International Journal of Heat and Fluid Flow. :.

December . -.

[] Y. R. Sivathanu and G. M. Faeth. "Generalized State Relationships for Scalar Properties in Non-Premixed

Hydrocarbon/Air Flames". Combustion and Flame. . –. .

[] Skjaeveland, S.M., Siqveland, L.M., Kjosavik, A., Hammervold Thomas, W.L., Virnovsky, G.A. . “Capillary

Pressure Correlation for Mixed-Wet Reservoirs”. SPE Reservoir Eval. & Eng.. . (). February, .

[] I. B. Sladkov. "Physicochemical Properties of Methyl- and Ethylhalosilanes". Russian Journal of Applied

Chemistry. . –. .

[] A. L. Smith. "Family Plots for Evaluating Physical Properties of Organosilicon Compounds". AIChE

Journal. . –. .

[] G. P. Smith, D. M. Golden, et al. "GRI-Mech . ". . http://www.me.berkeley.edu/gri_mech.

[] H. Smith, T. Lauer, M. Mayer, and S. Pierson . "Optical and Numerical Investigations on the Mechanisms

of Deposit Formation in SCR Systems". SAE Int. J. Fuels Lubr.. . . –. . DOI: ./-

.

[] P. L. Smith, Jr. and M. Van Winkle. "Discharge coefficients through perforated plates at reynolds

numbers of  to ,". AIChE Journal. (). –. .

.

[] D. O. Snyder, E. K. Koutsavdis, and J. S. R. Anttonen. "Transonic store separation using unstructured

cfd with dynamic meshing". Technical Report AIAA--. American Institute of Aeronautics

and Astronautics, 33th AIAA Fluid Dynamics Conference and Exhibit. .

[] G. Soave. "Equilibrium Constants from a modified Redlich-Kwong equation of State". Chemical Engin-

eering Science. . . .

[] G. R. Somayajulu. "Estimation Procedures for Critical Constants". J. Chem. Eng. Data. . –.

.

[] K. Stueben. "Introduction to Algebraic Multigrid". Multigrid. C. W. Oosterlee, U. Trottenberg, and A.

Schuller, editors. Academic Press, New York. –. .

[] Y. Sun, B. Vernham and S. A. Drenna. "Demonstration and Validation of Urea Deposit Predictions on

a Practical Mid/Heavy Duty Vehicle Aftertreatment System". ILASS-Americas 29th Annual Conference

on Liquid Atomization and Spray Systems. Atlanta, GA2017.

[] K. Sutton and P. A. Gnoffo. "Multi-component Diffusion with Application to Computational Aerother-

modynamics". AIAA Paper -. AIAA. .

[] M. Syamlal, W. Rogers, and T. J. O’Brien. MFIX Documentation: Volume , Theory Guide. DOE/METC-

, NTIS/DE9400087 National Technical Information Service, Springfield, VA. .

[] L. Talbot et al. "Thermophoresis of Particles in a Heated Boundary Layer". J. Fluid Mech. (). –.

.

[] W. Tang and K. Brezinsky. "Chemical kinetic simulations behind reflected shock waves". International

Journal of Chemical Kinetics. (). –. February .

[] R. I. Tanner. Engineering Rheology. Clarendon Press, Oxford, rev. edition. .

[] R. Taylor and R. Krishna. Multicomponent Mass Transfer. Wiley, New York. .

[] C. Temperton. "Implementation of a Self-Sorting In-Place Prime Factor FFT Algorithm". Journal of

Computational Physics. . –. .

[] P. A. Tesner, T. D. Snegiriova, and V. G. Knorre. "Kinetics of Dispersed Carbon Formation". Combustion

and Flame. . –. .

[] K. W. Thompson. "Time Dependent Boundary Conditions for Hyperbolic Systems". Journal of Compu-

tational Physics. . –. .

[] K. W. Thompson. "Time Dependent Boundary Conditions for Hyperbolic Systems II". Journal of Compu-

[] V. Torczon. "On the Convergence of the Multidirectional Search Algorithm". SIAM J. Optimization. .

. –. .

[] H. Wagner. "Soot Formation in Combustion". In 17th Symp. (Int’l.) on Combustion. The Combustion

Institute. –. .

[] G. P. Warren, W. K. Anderson, J. L. Thomas, and S. L. Krist. "Grid convergence for adaptive methods".

Technical Report AIAA--. AIAA10th Computational Fluid Dynamics Conference, Honolulu,

HawaiiAmerican Institute of Aeronautics and Astronautics. June .

[] E. W. Washburn. “Note on a Method of Determining the Distribution of Pore Sizes in a Porous Material”.

Proc. National Academy of Science. . . –. .

[] J. M. Weiss. "Calculations of Reacting Flowfield Involving Stiff Chemical Kinetics". AIAA--.

January .

[] J. M. Weiss, J. P. Maruszewski, and W. A. Smith. "Implicit Solution of the Navier-Stokes Equations on

Unstructured Meshes". Technical Report AIAA--, 13th AIAA CFD Conference. Snowmass, CO.

July .

[] C. Westbrook and F. Dryer. "Simplified Reaction Mechanisms for Oxidation of Hydrocarbon Fuels in

Flames". Comb. Sci. Tech. . –. .

July .

[] D. C. Wilcox. Turbulence Modeling for CFD. DCW Industries, Inc., La Canada, California. .

[] G. Zheng. "CFD Modeling of Urea Spray and Deposits for SCR Systems". SAE Technical Paper --

. .

[] V. Zimont, W. Polifke, M. Bettelini, and W. Weisenstein. "An Efficient Computational Model for Premixed

Turbulent Combustion at High Reynolds Numbers Based on a Turbulent Flame Speed Closure". J. of

Gas Turbines Power. . –. .

[]  Driver, D.M., (): "Reynolds Shear Stress Measurements in a Separated Boundary Layer Flow",

AIAA 22nd Fluid Dynamics, Plasma Dynamics and Laser Conference, AIAA--. .

[] F.R. Menter. "Two-Equation Eddy-Viscosity Turbulence Models for Engineering Applications". AIAA

Journal. (). –. August .

[]  Bell, J. H. & Mehta, R. D., (): "Development of a two-stream mixing layer from tripped and

untripped boundary layers", AIAA J., vol. , no., pp. -..

[] Vogel, J.C. & Eaton, J.K., (): "Combined Heat Transfer and Fluid Dynamic Measurements

Downstream of a Backward-Facing Step", Vol. , Journal of Heat Transfer, pp. – ..

[]  Bradbury, L.J.S., (),“The Structure of a Self-Preserving Plane Jet”, Journal of Fluid Mechanics

Vol. , pp.-. .

[] Wygnanski, I. and Fiedler, H.E., (),“Some Measurements in the Self-Preserving Jet”, Boeing

Scientific Research Labs, Document D1--. .

Part IV: Application Clients

The section describes how to use ANSYS Fluent application clients.

Remote Visualization and Accessing Fluent Remotely (p. ), describes the use of the ANSYS Fluent Remote

Visualization Client.

Fluent Icing (p. ), describes the use of the ANSYS Fluent Icing Client.

Chapter : Remote Visualization and Accessing Fluent Remotely

Using the ANSYS Fluent Remote Visualization Client you can start a visualization client session that can

be used to connect to up to six interactive or batch (Linux only) solver sessions on remote machines.

From the remote session you can:

Extract simulation data and visualize results using mesh, contour and vector plots.

Monitor solution convergence using residual and monitor plots.

Modify solution settings and start/pause/interrupt the calculation.

Send any text command to the server.

.. Starting Remote Visualization

If you have multiple releases of ANSYS products installed on your machine(s), ensure that the server and the

remote visualization client are from the same release, to avoid any unexpected behavior.

... Steps for Starting the Server

Before you start and connect a remote client session, the server has to be running.

. Start the server in the ANSYS Fluent session.

a.

b. Start the server.

File → Applications → Server → Start...

. Specify the name of the server info file and its storage directory. The default name of server_info-

<host process ID>.txt is supplied.

Note

For clusters with isolated compute nodes (for example, a Cray system) you must use the

export REMOTING_SERVER_ADDRESS environment variable to provide an outward facing

IP address for the client to connect to. This environment variable must be defined on both

the server and the client.

Alternate Methods for Starting the Remote Visualization Server

Here are a few more ways that you can start a server session.

The -sifile=server_info_example_name.txt command line startup option.

Note

sifile=D:/example_folder/server_info_example_name.txt. If you do

not provide a file path before the file name and you do not provide a path using the

SERVER_INFO_DIR environment variable, then the file is saved in your working directory.

From progress bar by clicking Start Server.

Figure . : Progress Bar with Start Server Option

Launch Fluent Remote Visualization Client from the start menu. Right-click the RemoteSession- branch

of the tree and select Start Server.

Enter the server/start-server text command into the console of a running Fluent session.

.... Port Management

When launching the server, you have the option specify a range of ports. There must be at least two

ports available from the range you supplied for the server to start, otherwise it will not launch. Note

that using this environment variable is optional, so if it is not declared, the server uses random ports.

Use the REMOTING_PORTS environment variable to specify the ports for starting the server: REMOT-

ING_PORTS=<start port>/portspan=<num>

<start port> and <num> must be valid integers

<num> must be greater than

<start port> must be greater than

Example:

If you specify REMOTING_PORTS=/portspan=, then only  ports are available: , ,

.

Each server requires two ports, so  and  are consumed when you launch the server. If you

Example:

.

then try to start another server on the same machine, it will not start as there is only one port ()

... Steps For Starting the Remote Visualization Client

. Start the server in the ANSYS Fluent session, as described in Steps for Starting the Server (p. ).

. Start the Remote Visualization Client ( options):

Scenario—Remote Client is on a different machine than the server.

Remote Visualization and Accessing Fluent Remotely

a.

(Windows) Launch Fluent Remote Visualization Client from the start menu.

(Linux) Launch the Fluent Remote Visualization Client from installation_drive/Program

Files/ANSYS Inc/v195/fluent/bin/flremote.

b. Click in the Server Info Filename field (highlighted in yellow in the Properties window), then click

Browse....

c.

Select the server information file and click Open.

d. Connect to the server session by clicking Connect in the Actions ribbon tab (Connection group

box).

Actions → Connection → Connect

Scenario—Remote Client is on the same machine as the server.

Start the remote client from the server session.

File → Applications → Visualization Client

The client will automatically connect to the server by loading the Server Info Filename.

Note

Important

The client and server machines must be able to connect by using their IP addresses. You

Important

can confirm that the machines can connect using IP addresses by ensuring that the ping

command works from both server to client and client to server.

Alternate Methods for Starting the Remote Visualization Client

You can start the client from progress bar by clicking Start client.

Figure . : Progress Bar with Start Client Option

Start Client will only appear as an option when there is not a Remote Visualization Client already con-

nected to the server.

Enter the server/start-client text command into the console of a running Fluent session.

Starting Remote Visualization

.. Using a Job Scheduler with Remote Visualization

You have the option to use job schedulers in coordination with the Remote Visualization Client and

server. Job schedulers are primarily covered in Setting Parallel Scheduler Options in Fluent Launch-

er (p. ), however, there are some nuances for using a job scheduler with remote visualization.

There are three types of server-client connections that you can make:

Start the client and server separately

Start the client from the server

Start the server from the client

The only type of connection that may require an additional step for remote visualization is when starting

the server from the client. For this case you must define the SERVER_INFO_DIR environment variable

on both the server and the client machines. Set the environment variable to a location that is accessible

for both the server and the client.

(Linux only) Fluent automatically selects the best graphics driver and defaults to using the X11 graphics

driver when it does not detect the required graphics support. You can use the HOOPS_PICTURE envir-

onment variable to force a particular graphics driver, if you feel it is necessary to use an alternate driver.

Note

SGE does not support starting the server from the client.

.. Operating in the Fluent Remote Visualization Environment

Once you are in the Fluent Remote Visualization Client you can display mesh, contours and vectors,

modify solution settings (as long as the server is not calculating), start, pause, and interrupt calculations,

and send commands.

... Adding New Remote Client Connections

From within a connected remote client session you can connect to up-to  other servers (a single remote

client can be connected to a maximum of  servers).

. Click New Connection... in the Actions ribbon tab (Connections group box).

Actions → Connection → New Connection...

This creates a new branch in the tree for the new remote session connection.

. Connect to the new server—two scenarios:

Connect to an already-running Fluent server

a.

Select the newly created sub-branch in the tree.

c.

box).

New server on the same machine as the client

a.

Right-click the new sub-branch in the tree and select Start Server.

b. Specify the appropriate settings in the Fluent Launcher and click OK to launch ANSYS Fluent. The

new Fluent session is automatically connected to the client.

... Initializing, Starting, Pausing, and Interrupting the Calculation

You have the ability to initialize, start, pause, and interrupt a calculation from the Remote Visualization

Client. The buttons for these actions are located in the Actions ribbon tab.

Initialize—fills the flow field with an initial "guess" for the solution.

Calculate—begins the process of Fluent calculating the solution.

Pause—"pauses" the calculation at the end of the iteration and waits for your input.When you click Resume,

Fluent continues calculating from where it was paused.

For example, if you request  iterations and pause at the 4th iteration, when you click Resume,

Fluent will calculate for the remaining  iterations.

If you are running from a script/journal file, Pause just "pauses" the run and all remaining commands

will be executed when you click Resume.

Note

Do not switch from steady-state to transient (or visa-versa) or change models when the

calculation is paused.

Resume—continues Fluent calculating the solution from the point where it was paused.

Interrupt—stops the calculation and takes the solver out of the iteration loop.You must then click Calculate

after adjusting the remaining iterations/time-steps.

For example, if you request  iterations and interrupt at the 4th iteration, when you click Calculate,

Fluent will calculate for  additional iterations ( iterations total).

If you are running from a script/journal file, Interrupt will cancel the run and the remaining commands

will not be executed.

Operating in the Fluent Remote Visualization Environment

Figure . : Actions Ribbon Tab

Select the Run Calculation branch in the tree to modify the Properties of RemoteSession-X: Run

Calculation.

Figure . : Run Calculation Properties

Important

Do not start calculations from the Send Command to Server dialog box—they must be

started using the GUI on the client.

... Modifying Solution Settings

When calculations are stopped or paused, you can modify solution methods, solution controls, and

convergence criteria from the Remote Visualization Client.

To modify the solution methods or controls:

. Select Methods or Controls in the tree. This opens the Properties of Remote Session-X: Methods or

Properties of Remote Session-X: Controls.

Figure . : Example Solution Methods

Figure . : Example Solution Controls

. Modify the solution methods and controls as required. Modified settings are automatically synched with

the server.

To modify convergence conditions:

. Select Residuals in the tree. This opens the Properties of Remote Session-X: Residuals or Properties of

Remote Session-X: Controls.

Figure . : Example Residuals Properties

. Modify the convergence conditions as required. Modified settings are automatically synched with the server.

... Graphics Objects

The remote client can access, display, and edit graphics objects that are defined on the server. You

can also create local graphics objects on the client.

The following sections describe operations available for graphics objects in the Fluent Remote Visual-

ization Client.

.... Creating and Displaying Graphics objects

.... Modifying the Views

.... Synchronizing with the Server

. Click New Mesh..., New Contour... New Vector..., New Pathlines..., or New Particle Tracks... in the

Actions ribbon tab (Graphics group box).

Actions → Graphics → New Mesh... | New Contour... | New Vector... | New Pathlines...

| New Particle Tracks...

You can also create new graphics objects by right-clicking Meshes, Contours, Vectors, Pathlines, and

Particle Tracks in the tree and selecting New....

. Specify all of the required fields in the Properties of RemoteSession-X: <graphics object name>.

Figure . : Example Graphics Object Properties

. Click Display in the Actions ribbon tab (Graphics group box).

Note

You can remove a graphics object from the remote client session by right-clicking it in the

Outline View tree and selecting Remove.

You can change how graphics objects are displayed in the graphics window of the Remote Visualization

Client directly in the graphics window and via the Viewing ribbon tab.

Figure . : Viewing Ribbon Tab

When changes are made to graphics objects on the server or the client, there are options (available

on a right-click of the object in the tree) to:

Send to server

sends changes made to the selected graphics object in the client to the server.

Retrieve from server

updates the graphics object in the client to match the state of the same object on the server.

View differences

prints the differences between the server and client versions of the graphics object to the console.

Arrows next to the graphics object indicate the state of the object. A single upward-pointing arrow

(

) indicates that this graphics object is unique to the client. A downward-pointing arrow paired with

an upward pointing arrow (

) indicates that the same object has different properties between the

server and the client.

Note

Changes (new graphics objects and modified object settings) sent from the client to the

server while the server is solving may not appear in the server until after the solving

completes.

... Messaging and Text Commands

Fluent communicates with you when you are in the Remote Visualization Client through messages

printed in the Console and the RemoteSession-X tabs. Generally, contents printed in the Console

tab are related to the remote client session, but not necessarily to a specific remote server connection,

whereas the RemoteSession-X tab(s) only apply to the server session that they are connected to. It

is important to check both messaging tabs to ensure that you are getting all the information Fluent

is sharing with you. The Console is also a Python . interpreter—refer to Python, Scripting and

Transcripts in the Remote Client (p. ) for additional information.

There are two ways that you can enter text commands from the Fluent Remote Visualization Client.

Through the console—only controls the client session (no effect on the server) and provides options to

exit the session and modify the views.

Through the Send Command to Server dialog box—sends commands to the server.This option offers all

of the commands listed in the Fluent Text Command List.

Important

Note

If the server is running with the active GUI present, some commands, such as changing

the discretization scheme, may require a refresh of the task page displaying the effected

field on the server (Solution Methods in the example of a modified discretization scheme)

before the change appears in the GUI—the changed field is still applied even if you do

not update the GUI display.

To send text commands to the server:

. Open the Send Command to Server dialog box by clicking Send Command... in the Actions ribbon tab

(Connection group box).

Actions → Connection → Send Command...

. Enter the text command into the Command text entry box.

Note

If you want the text command to be run in the background without the client waiting

for it to complete, then you can add an & to the end of the command. For example,

define/units velocity cm/s .&.

Figure . : Example of Sending a Command: Changing the Velocity Units to cm/s

. Click Send.

Important

While Fluent is solving, do not enter any commands that modify Fluent, such as changing

equations, plots, models, and so on, as this could cause errors.

Ensure that you only enter complete TUI commands in the Send Command to Server dialog

box.

box.

Confirm that you are sending the command to the intended server if you are connected to

multiple servers.The remote session that is sending the command is listed under Remote Session

Name. Select a remote session in the tree to review its properties, which includes the name of

the host machine (server).

As noted in the Warning dialog box that appears, commands are executed immediately in the

solver session without confirmation.This could cause a loss of work, if other users are connected

to and modifying the same session as you.

For any actions sent from the Remote Visualization Client to the server (initialization, starting

calculation, text commands using Send Command to Server), text prompts are automatically

answered. For example, if the question is The current data has not been saved. OK to discard?

ANSYS Fluent automatically answers OK to this question and begins calculating.

... Saving Case and Data Files

You can write case and data files from the client.

Actions → Connection → Write Case... | Write Data... | Write Case & Data...

Figure . : Writing Case and/or Data from the Client

Writing a case and/or data file:

. Click Write Case..., Write Data..., or Write Case and Data....

. Enter the name and location where the file(s) will be saved in the File name field.

. (Optional) Enable Write binary files to write binary files instead of text files. Binary files take up less space

and Fluent can read them and write them faster than text files.

. (Optional) Enable Overwrite file if exist if you want Fluent to write the new case and/or data files, even

if this means overwriting existing files with the same name in the location that you specified.

. Click Write to save the file(s).

... Disconnecting the Server and Client

If you want to break a server-client connection you can accomplish this in two ways: from within the

client and from within the server.

Note

If the server is closed unexpectedly, for example, the process is ended from the Windows

Task Manager, the remote visualization client may appear to hang, however after a time

out the client will become responsive again.

.... Disconnecting from Within the Remote Client Session

To disconnect from within the client:

. Select the RemoteSession-X connection that you want to break in the tree.

. Click Disconnect in the Actions ribbon tab (Connection group box).

Actions → Connection → Disconnect

You can also disconnect the session by right-clicking the RemoteSession-X branch in the tree and

selecting Disconnect.

Important

Do not try to close the server via the exit command in the Send Command to Server

dialog box, the correct command is (exit-server).

.... Disconnecting from Within the Remote Server Session

To disconnect a client from within the server you must shutdown the server.

Shut down the server by selecting Shutdown Server in the File ribbon tab.

File → Applications → Server → Shutdown

You can also shutdown the server by entering the server/shutdown-server text command in the

console.

console.

.. Python, Scripting and Transcripts in the Remote Client

This section is split into the following parts:

... Python Scripting

... Starting and Stopping a Transcript

Python commands allow you to query and/or modify some of the solution settings in the remote

session, create new graphics objects, and so on. You can also execute commands to initialize the

solution or calculate in the connected Fluent session. A Python script allows you to accomplish these

same operations by loading a script at startup or through the ReadScriptFile command (as shown

in Python Scripting (p. ).

There a multiple ways that you can load a Python script into the Remote Visualization Client:

At startup, using the -R command line option:

flremote -R <scriptName>

Through the File menu:

File → Read Script File...

Through the remote client console:

ReadScriptFile(ScriptFile = "filename")

The console in the Remote Visualization Client can be used as a Python . interpreter. You can import

any standard Python module and install new modules.

Your model in Fluent is stored in a hierarchy of Model State Objects. Model State Objects provide

functionality to access or modify problem settings.

The types of Model State Objects:

Parameter—lowest level object, which is used for storing strings, integers, doubles, and so on.

Singleton—container object that holds a set of child Model State Objects (which can be of any type).

Named Object—container object that holds a set of child Model State Objects and is used when many

objects of the same type can exist at a particular level. For example, the top-level RemoteSession object.

An instance of RemoteSession exists for every remote session that is created.

A RemoteSession object is pre-populated in the Python console. Settings for a specific session can

be accessed via the RemoteSession["<session-id>"] object.

Action

Method

Gets the child names of obj

obj.getChild-

Names()

For a Singleton object, it returns the child Model State object named "child".

obj.child

For a Named Object, it returns the Model State child object with a display

name or internal name of "name".

obj["name"]

For a Named Object, if a child with the name "name" does not exist, create

it. Set the child object state to state.

obj["name"] =

state

Iterator interface: Allows you to loop through the Named Object children of

obj and do some action on the children.

for child in obj:

do_some-

thing(child)

Check if childName is a Named Object child of obj.

if childName in

obj: do_something

Delete the Named Object with name "name".

del obj["name"]

State Access and Modification

Return the current state of the object. For container objects, a Python

dictionary is returned.

obj.getState()

Set the current state of the object. For container objects, state will be a

Python dictionary with the keys corresponding to the child object names.

obj.set-

State(state)

Same as obj.getState().

obj()

Same as parentObj.obj.setState(state).

parentO-

bj.obj=state

Return the internal name of the object.

obj.name()

Return the user-specified name of the object.

obj.displayName()

Commands

Get a list of available commands that can be executed on the object.

obj.getCommands()

Commands

Execute the command "command" with the specified arguments

obj.command(arg1

= value1, arg2 =

value2, ...)

Print a basic help about arguments for the specified command. If there are

no arguments, nothing is printed.

obj.command.help()

Important

Python commands that modify the Fluent application should be read from a script file using

the File/Read Script File... menu option. This allows for each command to complete before

the next command is executed. This is especially important for interdependent commands.

Typing or pasting a series of Python commands directly into the Remote Client console could

result in undesirable behavior as there is no waiting for the previous command to complete

before the next command is executed.

Note

Only a small subset of Fluent settings or actions are exposed in the scripting layer.

Python, Scripting and Transcripts in the Remote Client

While a script is executing, functions like Calculate() will wait for the command to complete

(whereas the calculation is done in the background if the same command is entered by typing

in the console).

Sample Script

The following example is a simple script that connects to session , reads a case (elbow) into the

server, initializes, modifies the under-relaxation factor for pressure, specifies the number of iterations,

then begins calculating. Once the calculation is complete, it creates and displays a pressure contour

plot of the results.

session1 = RemoteSession['RemoteSession-']

session1.ConnectionInfo.ServerInfoFilename = "server_info.txt"

session1.Connect()

session1.SendCommand(CommandName = "/file/read-case elbow.cas.gz")

session1.Case.Solution.Calculation.Initialize()

session1.Case.Solution.Controls.UnderRelaxationFactors['Pressure'].Value = .

session1.Case.Solution.Calculation.NumberOfIterations =

session1.Case.Solution.Calculation.Calculate()

session1.Case.Results.Graphics.createChild("Contour", "contour-")

session1.Case.Results.Graphics.Contour['contour-'].Field = "pressure"

session1.Case.Results.Graphics.Contour['contour-'].Surfaces = ['inlet1', 'inlet2', 'outlet', 'wall']

session1.Case.Results.Graphics.Contour['contour-'].Display()

Refer to the Python . documentation to learn more about working with Python.

The transcript feature allows you to save the output of the main Remote Visualization console into a

file, which includes the operations that you perform through the GUI.

You can start and stop recording a transcript through the File menu:

File → Start Transcript...

File → Stop Transcript

Or you can use the following Python commands entered into the remote session console to accomplish

the same:

StartTranscript(TranscriptFile = "filename")

StopTranscript()

.. Remote Visualization Best Practices

This section is a compilation of best practices for remote visualization.

The remote client immediately fetches data from a running (not solving) Fluent server session. However,

when the solver is running the client cannot fetch data immediately.The remote client can only communicate

with the solving Fluent server when the current iteration is over. For example, if an iteration takes  seconds,

then the remote client will take at least  seconds to fetch the data after you make the request.

While a remote client can connect to multiple Fluent server sessions, for best performance you should try

to have the connected server machines be running simulations that take a similar amount of time for calcu-

lating.

If a machine has multiple IP addresses, you should set the REMOTING_SERVER_ADDRESS to an outward

facing IP address, both on the client and server machines so that they can communicate with each other.

By default, both the remote client and Fluent server session have a  minute timer for completing a commu-

nication between the two machines. If the communication is not completed within the  minutes, then the

remote client and the Fluent server will disconnect from each other.You can reconnect the session. If the

communication timeout persists, you can control the timeout by setting the REMOTING_CONNEC-

TION_TIME_OUT environment variable.

For better performance, you should disconnect the Remote Visualization Client from the Fluent server session,

if you are not actively monitoring the solution on the client.

.. Remote Visualization Client Environment Variables

In certain circumstances you may have to change certain settings that are controlled by environment

variables. Table . : Remote Visualization Client Environment Variables (p. ) lists all of the environment

variables that are specific to the Fluent Remote Visualization Client and their uses. You can define the

environment variables in the Environment tab of the Fluent Launcher.

Table . : Remote Visualization Client Environment Variables

Input & Use

Variable

time in seconds

REMOTING_CONNECTION_TIME_OUT

It is used to define the time out for requests from client

to server and visa-versa. The default value is

seconds ( minutes). If a request is not completed by

the server within this time, then the client will show

an error.

<folder path>/<file name> for example,

E:/Testing/remoting/example_log

REMOTING_LOG_FILE

It is used to define the log file path. If this variable is

defined, then the client and server will write log files.

size in bytes

REMOTING_MAX_MESSAGE_SIZE

It is used to define the maximum message size that

the client and server can exchange.

<start port>/portspan=<num>

REMOTING_PORTS

It is used to define the port range. If this variable is

defined, then the remote client will try to start the

server within the specified port range.

Public facing IP address

REMOTING_SERVER_ADDRESS

It is used to define the server's IP address. If this

variable is defined, the remote client will not identify

the IP addres; it will use the provided address instead.

The address will be written to the log file. Define this

environment variable if the machine has multiple IP

Remote Visualization Client Environment Variables

Input & Use

Variable

addresses or if the Remote Client is unable to resolve the

IP address.

While a remote client can connect to up to  different remote Fluent server sessions at once, a single server

can only have one remote client connected at a time.

You cannot rename or delete graphics objects from the remote client

(Windows only) Starting the server is not supported if ANSYS Fluent is launched with either the -g or -gu

options from the command line.

If a calculation is started on the server-side, the beginning and end of the transcript will be missing on the

client-side.

For any actions sent from the Remote Visualization Client to the server (initialization, starting calculation,

text commands using Send Command to Server), text prompts are automatically answered. For example,

if the question is A report file already exists with this name in the current directory. Create a new report file?

ANSYS Fluent automatically answers yes to this question and begins calculating.

Do not start calculations from the Send Command... option on the client side- they must be started using

the GUI on the client.

Plot properties (that is, axis and curve properties) are not transferred to the Remote Visualization Client.

Residuals are always plotted on a logarithmic scale and other plots are on a standard scale.

Report plots cannot be created or edited from the Remote Visualization Client.

(Linux only) If a Remote Visualization Client is started from a server, the client will close when the server that

launched it is closed.

Custom mesh colors can only be set in the server, although they can still be displayed in the client.

When running in parallel, mesh partitions can only be displayed on the server. If you have a mesh

object with Partitions enabled and you display that mesh object on the client, you will not see the

mesh partitions due to this limitation.

Differences between graphics objects on the server and the connected client will not appear if the

displayed options are not available on the client. For example, if you enable Partitions in a mesh

object on the server, it will not appear as having changed on the client.

Mesh motion preview will not update automatically on the client. Client mesh displays are only updated

when you click Display.

Symmetry, Mirror Planes, and Periodic Repeats displays are not supported on the client.

User-defined colormaps are not available for the client. Any objects on the server using a user-defined

colormap will not display on the client.

Commands that modify the state of the server (such as initialization), retrieve the latest solver settings

when they are sent to the server using the Send Command to Server dialog box. This could result

in, for example, the number of specified iterations on the client changing to match the number of

iterations specified on the server.

Addon modules are not supported with the remote client. If you have an addon module enabled on

the server, information regarding the addon module will not be shown on the client. For example,

Adjoint residuals will not display on the client.

The client cannot display more than  windows. If you have more items to plot than , consider

including multiple report definitions within a single report plot to reduce the number of windows.

You can also deactivate report plots to allow for new plots without deleting the existing plots.

To reset the graphics window layout in the client you must delete the .flremote.layout file

from the operating system home directory, then close and reopen the remote client.

Zoom-to-fit does not work on the remote client when the server is iterating. You can pause the cal-

culation to use the zoom-to-fit functionality.

If the Reporting Interval in the Run Calculation task page is set to a value greater than , residuals

plotted on the remote client will respect that reporting interval and will therefore not appear precisely

the same as the residuals plotted on the server.

Using a virtual private network (VPN) for remote visualization may not work in some situations due to certain

firewall security measures in place at the server site. Any disruption in the VPN and/or internet connection

may cause an unexpected failure.

The viewing and display options available in the remote client are based off of the dimensions of the

most recently connected remote session. For example, assume your remote client is connected to

two servers, one 3D and one 2D, and the 2D session was connected second. The available display

options in the client will reflect the available options for the 2D session, even if you are trying to

visualize on the 3D session. To remedy this issue, you can disconnect and reconnect the 3D session,

which will make all of the 3D-related display options available in the client.

Chapter : Fluent Icing

The following sections of this chapter are:

.. Overview of Fluent Icing

.. Quick Start

.. Launching Fluent Icing

.. Fluent Icing Graphical User Interface Layout

.. Creating a Fluent Icing Simulation

.. Setting-Up a Fluent Icing Simulation

This document provides some basic guidelines on how to simulate in-flight icing conditions using Fluent

Icing. Fluent Icing unifies CFD simulation of air flow with in-flight icing physics in a single-window, in-

tegrated workflow.

Fluent Icing incorporates the three principal aspects of in-flight icing simulations, airflow, particles

(droplet and ice crystal impingement limits and shadow zones), and ice accretion. It has no geometric

limitations and is applicable to aircraft, UAVs, nacelles, probes, detectors, etc.

Important

The current version of Fluent Icing exposes only a subset of the full in-flight icing capabilities

and modules of FENSAP-ICE. In this version, the FENSAP-ICE modules exposed are, FENSAP

for airflow (as an alternative to Fluent), DROP3D for particles and ICE3D for ice. More complete

information regarding these modules can be found in the FENSAP-ICE online documentation.

The following types of icing analysis can be performed with the current release of Fluent Icing

Particles

– Standard droplets, SLD (break-up, splashing and bouncing) and crystals

– Transport of vapor

– Appendices C, O and D icing environments

– Predefined droplet size distributions

Langmuir A (Monodispersed) to E

Ice

– Rime, glaze and mixed icing calculations

– Single & multiple quasi-steady shots called multishots

– Automatic mesh deformation during multishot calculations

Ice

Note

A complete work procedure, with example datasets and conditions is available under Fluent

Icing in the Fluent Tutorial Guide.

To set-up a case for icing

Open the Fluent Icing application. In Windows, go to the Start menu and select Fluent Applications →

Icing. In Linux, launch icing from the fluent/bin directory.

Go to File → Open Case... and select a suitable case (.cas, .cas.gz, .cas.h5) file, provided with a Fluent

airflow converged solution alongside it (.dat, .dat.gz, .dat.h5).

Note

The case must contain a 3D mesh without polyhedral or adapted elements. The reference

conditions and material type (Air) should be suitable for icing conditions.

When prompted to Launch Fluent, select Yes. Fluent is launched with the default number of CPUs () set

in Preferences.

Once Fluent is connected, use the icing application to review the conditions and solver settings:

– Set-up → Airflow

Review the airflow conditions and configure them if necessary.

– Set-up→ Particles → Droplets

Set the conditions and default settings, which will be used for the particles simulation.

– Set-up → Ice

Set the conditions and default settings, which will be used for the ice simulation.

– Set-up → Boundary Conditions → wall-, wall- wall-, wall-

Set temperature to Adiabatic +  by right-clicking the icon of the walls subject to icing. Double-

click on each wall and activate High roughness for Icing in Wall Roughness within the Properties

window.

In Outline View → Solve:

window.

– The Airflow node is shown with a green check mark, indicating that an airflow solution was loaded and

is ready to use.

– In the Solve → Particles node, the number of iterations for the Particles solver can be configured.

Fluent Icing

→ Right-click on Particles, and choose Calculate.

→ The Particles solver runs and produces a droplet solution.

– Use the ribbon and click on View → Contour → Collection efficiency – walls option to view the water

catch on the walls, the solution is displayed in the Graphics window.

– In the Solve → Ice node, the total time of ice accretion can be configured.

→ Right-click on Ice, and choose Calculate.

→ The Ice solver runs and produces an ice solution, which is composed of scalar values on walls and the

ice shape.

– Use the ribbon and click on View → Ice cover options to view the scalars of the ice solution as well as

the ice shape using CFD-Post or Viewmerical.

The Fluent Icing application can be started from either:

Your ANSYS installation folder

– Windows

fluent/bin/icing.bat in Fluent folder.

– Linux

fluent/bin/icing in the Fluent folder.

Your ANSYS Start menu in Windows

Fluids → Fluent Applications → Icing in the ANSYS Start menu entry.

An existing Fluent session, where an airflow case is loaded and ready to simulate ice accretion.You can

either launch Fluent Icing using the same machine as your Fluent session or another machine.

– To launch Fluent Icing from the same machine

File → Applications → Icing This will open the Fluent Icing window and will run Fluent Icing on

the same machine as your Fluent session.

– To launch Fluent Icing on a different machine

File → Applications → Server → Start. Select Icing in the pop-up window and save a server-info

file. Start Fluent Icing (on any other machine), then use File → Connect to... to connect to the

running Fluent server, by using the server info file.

Note

Network limitations or firewall might affect the ability to connect from a remote machine.

Launching Fluent Icing

If the Fluent Icing application was loaded first, closing the Fluent Icing application will

automatically close its connected Fluent session. If Fluent Icing was started from Fluent

itself, or connected via the Connect to… menu, closing the Icing application will not close

Fluent automatically.

Figure . : The Fluent Icing Graphical User Interface

The Fluent Icing graphical user interface (Figure . : The Fluent Icing Graphical User Interface (p. ))

consists of the following components

File (Top-Left)

Consists of file management commands (Open Case, Save, etc.)

Ribbon (Top)

Provides access to

– Set-up

→ Some file management commands

→ Special icing conditions settings

– View

→ Post-processing commands and quick-view actions

Outline View (Left)

Contains a list of currently open cases. Each case is connected to a Fluent session and provides access

to

– Set-up

Model and conditions settings for each module of the icing sequence

– Solve

Execution controls of the solvers

– Results

Post-processing data

Properties window (Center)

Contains the settings of a selected item in the Outline View.

– Solve

– Results

Graphic windows (Right)

Displays mesh, numerical, postprocessed and monitoring data.

Console window (Bottom)

Displays the progress of your simulation and allows scripting of commands. The default console is a

Python console.

Note

In the case of Fluent sessions, each session has a separate console window, which displays

the fluent execution log. This console cannot be used for commands. To send a text

command to Fluent, right-click on the Fluent case in the Outline View and choose Send

Command...

File Menu

Open Case

Fluent Icing Graphical User Interface Layout

Select a case file and open this case in a Fluent session, see Loading a Case File (p. )

Connect to...

Connect to an existing Fluent session, see Launching Fluent Icing (p. )

Save Case

Save current case file at its current location

Save All

Save case file and all solution files alongside it

Save Case as...

Save case file and all solutions in a new location or with a new file name

Import

Select a case file or grid, and copy it to the current work directory, then open Fluent.

Export

– Write FENSAP grid...

Writes the current case file to a FENSAP-ICE grid file format

Read Script File...

Select a python script file to execute, see Python Commands (p. )

Preferences...

Opens the Fluent preference window. The Icing window is specific to the Icing Application. See

Preferences (p. ).

Exit

Exit the Icing application

All Fluent sessions will also be terminated unless the session was created via a Connect command,

or the Icing application was launched from Fluent itself)

Ribbon Commands

Set-Up

– Case

Set-Up

– Case

→ Open...

→ Import...

→ Save

→ Save all

→ Save as…

→ Check

Check the case and set-up for compatibility with Icing solvers. See Case File Requirements (p. )

– Conditions

→ Atmospheric

Opens cloud environment types to define droplets and crystals properties. See Particles (p. ).

→ Distribution

Displays and toggles between available built-in particle distributions. See Particles (p. )

View

– Quick-view

Access to post-processing shortcuts, see Quick-View (p. ).

– Graphics

Create new post-processing objects. See Basic Graphics Generation within the Fluent User's Guide.

Fluent Icing is mainly focused on computing particles and ice simulations from an airflow simulation

case file. Therefore, it is strongly recommended to set-up your Airflow case file in Fluent before

launching Fluent Icing. If available, an airflow solution (.dat) can also be loaded with the case file.

Note

To set-up a Fluent case file for icing calculations, please consult Recommendations to Set

up a Fluent Calculation.

Similar to the Fluent Remote Client, it is possible to add multiple cases, connected to local

or remote Fluent sessions. However, each loaded case requires a separate Fluent license &

CPUs

... Case File Requirements

CPUs

The Fluent mesh must respect the following properties:

3D only

2D Fluent mode is not supported. 2D geometries are supported via 3D meshes with symmetry or

periodic planes.

Grids with polyhedral elements or adapted grids with hanging nodes are not supported.

Grids must not have deactivated zones.

Boundary condition types cannot be changed inside Fluent Icing, therefore they must be properly set-

up before the case file is loaded into Fluent Icing.

... Loading a Case File

Upon startup, the Fluent Icing application has no case loaded and presents an empty Simulations

window.

The first step to set-up a Fluent Icing simulation is to either open or import a case file.

.... Opening a Case File

Set-Up → Open... selects a Fluent case file (*.cas, *.cas.gz, *.cas.h5). This operation will

prompt the user to launch Fluent. Fluent will be launched in a secondary window, once the connected

case file is loaded.

If a Fluent solution file (*.dat, *.dat.gz, *.dat.h5) is alongside the case file, it will be also

loaded.

Yes

Fluent is launched on the current machine, using the default options inside Preferences.

Note

The default MPI type, and 3d double-precision solvers are automatically used.

Fluent is launched in a separate window, minimized upon start-up. On some Windows

managers, the window might not minimize and Fluent will open over the Fluent Icing

window. You can switch back to the Fluent Icing window once the case file is loaded.

No

Fluent launch is delayed; the Fluent launch settings can be fine-tuned in the Properties of Case

window. Fluent can later be launched using the Start Fluent command as shown below.

No

Creating a Fluent Icing Simulation

Fluent Launch Settings

The default values for the launch settings are set in the Preferences window, see Preferences (p. ).

If the value is unsuitable for the current run, modify these values in the Properties of Case window

before launching Fluent.

Number of CPUs

The amount of MPI CPUs used to launch the Fluent and any other Fluent Icing solver. A suitable

license is required.

Use Fluent launcher

The Fluent launcher is displayed on Fluent start-up and the launch options and environment can

be fully configured (such as Job scheduler, remote launch options, environment variables, etc. ).

Below are the execution requirements inside Fluent Launcher:

– Dimension → 3D

– Options → Double Precision

This is strongly recommended for increased precision of mesh coordinates.

– Processing Options → Parallel

Serial is a deprecated feature not supported by the Fluent Icing Particles and Ice components.

CPU can also be used in Parallel mode.

Note

ACT and GPGPUs are not used by FENSAP-ICE, therefore not supported by Fluent Icing.

Only 3D meshes are supported.

.... Importing a Case File

Fluent Icing allows you to import (copy) case and mesh files to your Working directory.

Import Case – Fluent Case or Mesh

Using the Import case command, a Fluent case file (.cas, .cas.gz, .cas.h5) or mesh file

(.msh) can be selected. If an airflow solution (.dat) file exists in the same location with the same

root name as your case file, it will also be copied to your working directory. If the file is a .msh mesh

file, it will be copied as a .cas file.

Note

Fluent Icing does not offer the option to modify the boundary condition type. The

boundary conditions types need to be set-up beforehand in Fluent.

Import Case - FENSAP

Using the Import case command, a FENSAP format grid (*.grid) file can be selected. When

imported, the grid file is converted to Fluent case file format.

Note

All inlet surfaces are automatically set-up as pressure-far-field.

The air material properties and the energy / viscous models are set to the default recom-

mended values, see Recommended Settings (p. ).

Working directory

A working directory is an optional directory which can be used to store the case files currently worked

upon. If enabled, this directory will be used to import cases and used as the default current directory

for Fluent Icing calculations.

The working directory can be enabled and configured through the Preferences window under the

Icing category.

Once a case file is loaded, a simulation tree appears under your case file. This tree if composed of three

main components

Set-up, Solve and Results.

Set-up

Defines the type of simulation, the in-flight icing conditions, the physical models and the boundary

conditions to use in your simulation.

Solve

Defines the solver settings of your in-flight icing simulation including monitoring, initialization and

output files.

Results

Allows post-processing of your in-flight icing results.

... Set-up

Simulation Type

To start your simulation, you must define its type. Three types are provided in the Properties of Set-

Results

... Set-up

up window of the Set-up component.

Airflow

The airflow solver. Two solvers are supported (Fluent and FENSAP).

Particles

The particles impingement solver, in this case DROP3D. An airflow solution is required before con-

ducting this simulation.

Ice

The ice accretion solver, in this case ICE3D. An airflow and particles solution are required before

conducting this simulation.

Therefore, five combinations of simulation types are supported:

Stand-alone Airflow simulation

Stand-alone Particles simulation, with an airflow solution already loaded.

Stand-alone Ice simulation, an Airflow and Particles solution already loaded.

An Airflow + Particles simulation. Each simulation is run in sequence.

An Airflow + Particles + Ice simulation. Each simulation is run in sequence.This combination allows the

simulation of single and multiple quasi-steady (multishot) ice accretion calculations.

Disabling a Simulation type from the Properties of Set-up window of Set-up will hide its relevant

settings from the Outline View.

Example . : Some Settings Are Used by All Simulation Types and Will Be Displayed at All

Times

Airflow conditions are used by all  simulation types and Particle conditions are required for Ice.

Setting-Up a Fluent Icing Simulation

Global settings

Advanced features

Activates additional options within some Fluent Icing windows, see Advanced Settings (p. ).

Beta features

Activates Fluent Icing Beta features. Consult the Fluent Beta Features Manual for more information.

.... Airflow

The Properties of Airflow window defines the airflow solver, the airflow conditions and the direction

of the icing simulation.

General

Choose between Fluent and FENSAP as the Airflow solver. Your choice will appear in the Outline

View as an Airflow branch under Set-up. Clicking on this branch will allow the set-up of the air

properties and physical models of either Fluent or FENSAP.

These are the reference airflow conditions used by all simulation types. By default, its values are

copied from the Reference Conditions of the case file.

Sync with Fluent ref. conditions

If this option is enabled, any change in the Conditions window will be mirrored to the Reference

Conditions window of the Fluent window. If this option is disabled, these values are used only

inside Fluent Icing, and the Reference Conditions in the Fluent window will remain unchanged.

The parameters shown below Sync with Fluent ref. conditions mainly correspond to the reference values

described in FENSAP-Flow Solution →Flow Conditions → Reference Conditions of the FENSAP-ICE User

Manual. The table connects these variables to FENSAP-ICE or Fluent variables.

Fluent

FENSAP-ICE

Length

Characteristic length

Characteristic Length

Velocity

Air velocity

Speed

Air static temperature

Air static pressure (FENSAP

only supports absolute pressure

Relative Pressure

quantities). The Air static

pressure of FENSAP is the sum

of the Relative Pressure and the

Operating Pressure in Fluent

Icing.)

Note

Icing.)

Note

If you would like to use absolute pressures in Fluent Icing, set the Operating Pressure

to  Pa in the Properties of Airflow window. The Relative Pressure and Gauge Pressure

becomes the static pressure.

Direction

Two approaches to specify the orientation of the reference airflow is supported.

Cartesian components

The direction is specified by assigning velocity components in X, Y and Z.

Angle of attack

The direction of the flow is specified via two angles, AoA [deg.] and Yaw [deg.] and its velocity

magnitude by Velocity magnitude [m/s]. The planes on which these two angles are defined are

obtained by selecting the coordinate axis of lift (Lift Direction) and drag (Drag Direction) for a zero

degree AoA. The AoA is defined on the plane consisting of the Drag Direction as the primary axis

and the Lift Direction as the secondary axis, while the Yaw angle is defined on the plane consisting

of the Drag Direction as the primary axis and the result of the cross product of Drag Direction x

Lift Direction as the secondary axis.

For instance, if the Drag Direction is set to X+ and the Lift Direction is set to Y+, the flow direction

will be defined by the X+ axis if you set the AoA [deg.] and Yaw [deg.] to  degree. If the AoA [deg.]

is set to  degrees and the Yaw [deg.] is set to  degree, the flow will be entirely in the Y+ direction.

If the AoA [deg.] is set to  degree and the Yaw [deg.] is set to  degrees, the flow will be entirely

in the Z+ direction.

Fluent Airflow Solver

If Fluent has been selected as the Airflow solver in the Properties of Airflow window, the following

Properties of Fluent window appears if you click on Set-up → Airflow → Fluent. In this window,

you can specify the material properties of air and the most common physical models of air used for

icing simulations.

For more information regarding recommendations on how to set-up air properties and physical

models in Fluent, consult Recommended Settings (p. ).

Materials

Set the same air properties as the ones coming from the loaded case file (Fluid set to Case settings)

or set new air properties (Fluid set to Air).

The parameters shown below Fluid are the Fluent parameters and they only appear if Fluid is set to

Air. Only Ideal gas and Constant properties are supported by Fluent Icing. Follow Recommended

Settings (p. ) to define the air properties for icing calculations.

Models

The parameters shown in Models are the Fluent parameters under Setup → Models. Only the phys-

ical models recommended in section Recommendations to Set up a Fluent Calculation of the FENSAP-

ICE User Manual are provided. Follow Recommended Settings (p. ) to select the appropriate models

for icing calculations.

The Other flag is displayed next to Turbulence when the case file contains a viscous model that is

different than the ones supported by Fluent Icing (k-Omega -eqn and Transition SST -eqn).

Although viscous heating and energy appear as options here to be compatible with standard Fluent

setup, they have to be enabled for icing simulations otherwise heat transfer coefficients used in the

ice accretion model will not be calculated correctly.

Commands

Access the following commands by right-clicking on Fluent, located in Set-up → Airflow → Fluent.

Set to default Air properties

Changes the current material to Air and will set the air material properties to the Recommended

settings, see Recommended Settings (p. ).

Set to default Models

Enable the Recommended settings for models. See Recommended Settings (p. ).

Update with Fluent settings

Use this option to synchronize your Fluent session changes with Fluent Icing.

Note

Changes made to Fluent Icing are automatically synchronized with Fluent.

Recommended Settings

When performing icing simulations using Fluent as the airflow solver, the following Material settings

for Air are recommended.

Set the Density - Option to ideal-gas

Set the Cp - Option to . J/kg/K.This value is equal to /, the gas constant R of .

J/kg/K.

Set the Thermal Conductivity - Option to Constant and set its Constant to an appropriate value for the

condition.To compute its value, refer to the thermal conductivity equation below.

Set the Dynamic Viscosity - Option to Constant, and set its Constant to an appropriate value for the

condition.To compute its value, refer to the viscosity equation below.

Use the following equations to compute the thermal conductivity and dynamic viscosity, respectively.

Furthermore, the following Model settings are recommended.

– Energy must be enabled for icing simulations.

– The Turbulence model K-Omega -eqn is recommended for icing simulations.

– Viscous Heating and Turbulence Production Limiter must be enabled for icing simulations.

FENSAP Airflow Solver

If FENSAP has been selected as the Airflow solver in the Properties of Airflow window, the following

Properties of FENSAP window appears if you click on Set-up → Airflow → Fensap. In this new

window, you can specify the most common physical models of air and options for artificial viscosity

used in icing simulations.

The most common airflow properties of FENSAP for icing simulations are the Ideal Gas properties

with constant thermal conductivity and dynamic viscosity as specified in the Recommended Set-

tings (p. ).

Model

In Fluent Icing, the Momentum equations are always set to Navier-Stokes and three options are

available for Energy.

Full PDE, Constant enthalpy and Energy only. Full PDE is the most common option for icing applic-

ations. By default, FENSAP solves the energy equation in non-conservative form which results in robust

convergence especially when the momentum and energy systems are uncoupled. To solve the energy

equation in conservative form, enable Conservative.

For more information regarding these settings, consult The Energy Equation.

All turbulence and transition models of FENSAP are supported in Fluent Icing. The default settings

(SA with no transition) are the most common for ice accretion simulations. For more information re-

garding these models, consult section Turbulent Flows and Transition to Turbulence.

Note

Default numerical convergence settings are applied to all turbulence models of FENSAP.

Note

Artificial Viscosity

All the artificial viscosity options of FENSAP are supported in Fluent Icing. The default settings

(Streamline upwind with second order cross-wind dissipation of 1e-) are the most common settings

to obtain an accurate and stable airflow solution with FENSAP. To improve the accuracy, you can reduce

the cross-wind dissipation as long as you are able to maintain a stable solution and a smooth distri-

bution of shear stresses and convective heat fluxes over the walls of your geometric model. For more

information regarding these artificial viscosity models, consult Artificial Dissipation.

.... Particles

The Properties of Particles window defines the type of particles to simulate and the activation of

the energy equation in the event that high temperature gradients might affect the local concentration

of these particles within the computational domain.

Note

The air and particles could be solved simultaneously (as a two-phase flow). However, since

the particles volume fraction is very small, the two-phase flow is considered a dilute gas-

particle flow and thus the governing equations of air and particles are solved in a segregated

manner. The airflow is solved first, followed by the particle equations. In this manner, the

effect of the air on the particles is considered, but not the reverse.

Type

Three particle types are supported:

Droplets

Supercooled water droplets that are still in liquid form at lower ambient temperatures. They typically

accrete on external aircraft surfaces.

Crystals

Crystals

Ice crystals are solid ice particles of various sizes that are suspended in air. They typically accrete

on internal aircraft surfaces where large temperature gradients are experienced.

Vapor

Water vapor is a substance in the gas phase. In icing modeling, its concentration can vary by mass

and energy transfer with droplets/crystals.

These particle types can be selected concurrently and thus they can all be simulated simultaneously

within the same Particle simulation.

Enabling a particle Type from the Properties of Particles window will create its corresponding branch

under Particles as well as any other relevant setting related to this particle type in Boundary Condi-

tions and Solve.

Model

By default, continuity and momentum equations of droplets and crystals, and continuity equations

of vapor are always solved when these particles are selected in Type. These are the typical equations

needed to study external in-flight icing physics. For more information regarding these equations,

consult The Particle Transport and Supercooled Large Droplets (SLD).

To activate the energy transfer between particles as well as their respective phase change, the Particle

thermal equation must be enabled. It is recommended to enable this option when studying internal

in-flight icing physics, e.g. inside engines.

Droplets

If Droplets has been selected as a particle Type in the Properties of Particles window, the following

Properties of Droplets window appears when you click on Set-up → Particles → Droplets. In this

window, you can specify the ambient/reference conditions of water droplets, the type and size distri-

bution, and the drag model.

Droplet conditions

The main physical parameters describing the droplets are:

LWC [kg/m3]

The Liquid Water Content (LWC) is the concentration of water droplets in the air.

Droplet diameter [microns]

Spherical droplets are assumed to be of a single, uniform size, usually equal to the median volume

diameter (MVD) of the sample size distribution. In Particles, the droplet diameter is the MVD.

Water density [kg/m3]

This is the density of the water droplets. By default, its value is set to , kg/m3.

SLD

Supercooled Large Droplets (SLD) options allow the set-up of extra physical models when water

droplets exceed a MVD of ~ microns.

Appendix conditions

Allows to set-up recognized cloud environment type conditions. In this case, droplet conditions

will be automatically defined based on flight conditions and droplet size. The following appendices

are supported

– Appendix C

In general, environment type for droplet sizes below  microns.

– Appendix O

In general, environment type for droplet sizes that exceed  microns.

For more information regarding these appendices, please consult Appendix C and Appendix O -

Supercooled Large Droplets.

Particle distribution

Only built-in droplet size distributions are currently supported by Fluent Icing. These distributions

can be selected in the Droplet distribution pull-down menu.

Monodisperse

Indicates that a calculation is performed using a single diameter. This diameter is specified in the

Droplet diameter box and corresponds to the MVD.

Langmuir B to E

If one of these is selected, water droplets are simulated by computing the droplet concentration

and speed for each individual diameter of the discrete distribution, which are subsequently auto-

matically weight-averaged at the end of the simulation. Fluent Icing always uses  droplet diameters

to represent a Langmuir B to E distribution. The various Langmuir diameter distributions and their

corresponding weights are pre-defined in FENSAP-ICE. To learn more about these distributions and

their respective weights, please consult Droplets Reference Conditions.

Model

In this submenu, different water droplet physical models can be enabled in order to increase the ac-

curacy of your water droplet simulation. Some of these models are only available when the SLD option

is enabled in Droplet conditions.

General Models

– Droplet drag model

These models correspond to drag correlations. Only  choices are available (Water, Water -Stokes

law, Water – extended Reynolds, Snowflakes). The default drag model is set to Water, which

is the drag model used in almost all our water droplet validation cases. For more information

regarding these models, please consult Particle Drag Correlations.

SLD only Models

– Break-up model

Models the process by which a large droplet is broken up into smaller droplets due to aerody-

namic forces. To enable this model, select Pilch & Erdman, the only break model supported in

FENSAP-ICE. If selected, an extra governing equation is solved for droplet diameter. For more

information regarding this model, please consult Droplet Break-Up.

– Splashing and bouncing

Only the By post-processing with three splashing models (Mundo, Honsek and Wright) are

supported in Fluent Icing. These are the most validated models used in SLD splashing & bouncing

simulations, with a preference for Mundo, default Splashing model setting. They modify the

droplet collection efficiency on the surface by predicting if water droplets bounce or splash.

Droplets that bounce or splash are not re-introduced into the computational domain. For more

information regarding these models, consult Splashing and Bouncing by Post-Processing, Mundo

Model, Honsek-Habashi Model and the Wright Potapczuk Model section within the FENSAP-ICE

User Manual.

– Terminal Velocity

This option enables SLD particles to fall without exceeding its terminal velocity (maximum fall

speed). This option will alter the transport of droplets and therefore its impingement. The direction

and the magnitude of the gravity vector must be specified in the case file. For more information

regarding this model, please consult Terminal Velocity.

Crystals

If Crystals has been selected as a particle Type in the Properties of Particles window, the following

Properties of Crystals window appears when you click on Set-up → Particles → Crystals. In this

window, you can specify the ambient/reference conditions of crystals.

Note

Note

Only one drag model of crystals has been implemented and it follows the oblate spheroidal

drag correlation formulated by Pitter. For more information regarding this model, please

consult Ice Crystal Drag Correlations.

Crystal conditions

The main physical parameters describing the ice crystals are:

Ice Crystal Content [kg/m3]

The Ice Crystal Content (ICC) is the concentration of crystals in the air.

Crystal diameter [microns]

Ice crystals are assumed to be of a single, uniform size. In this case, the crystal diameter corresponds

of the semi-major axis length of a thin oblate spheroid.

Crystal density [kg/m3]

This is the density of the ice that forms the ice crystal. By default, its value is set to  kg/m3.

Crystal Aspect Ratio

This is the aspect ratio (E=b/a) of an oblate spheroid, where b is the semi-major axis length and a

is the semi-minor axis length.

Allows to set-up the recognized cloud environment type condition called Appendix D (crystals).

In this case, ice crystal conditions will be automatically defined based on flight conditions, the Total

Water Content (TWC = LWC + ICC) and the LWC, if droplets are present. For more information re-

garding Appendix D, please consult Appendix D - Ice Crystals.

Vapor

If Vapor has been selected as a particle Type in the Properties of Particles window, the following

Properties of Vapor window appears when you click on Set-up → Particles → Vapor. In this window,

you can specify the ambient/reference conditions of vapor.

The main physical parameters describing vapor are:

Relative Humidity [%]

This option is enabled if selected under Vapor initialization. This option corresponds to the ambient

relative humidity and ranges from  to  %. It is defined as the ratio of partial vapor pressure to

the saturation vapor pressure.

Vapor Concentration [kg/m3]

vapor concentration.

.... Ice

The Properties of Ice window defines the icing conditions and the icing physical models to use

during the ice accretion simulation.

Ice accretion conditions

The main physical parameters describing the ice accretion process are:

Recovery factor

The recovery factor is used to introduce the effect of the energy losses due to friction when com-

puting the adiabatic/recovery temperature at the wall. This is a factor that is used to compute the

convective heat transfer coefficients in FENSAP-ICE for ambient/reference or icing temperatures.

Its default value is . (~Pr1/), a value that has been used in several icing validation cases.

Icing air temperature [K]

The icing air temperature is the static temperature at which ice accretion is computed. This temper-

ature can thus be different than the ambient air temperature specified in the Properties of Airflow

window or inside your inlet boundary conditions. If the energy equation of particles is enabled,

the icing air temperature must be the ambient air temperature specified in the Properties of Airflow.

Relative humidity [%]

This is the relative humidity expressed in percentage value. For clouds, this value should be set to

%. If Vapor has been enabled in Particles, this parameter is disabled, and vapor distributions

are used inside the icing models.

For more information regarding these parameters, consult Icing Conditions.

Model

The main physical models describing the ice accretion process are

Icing model

The icing models solve the SWIM equations (see Governing Equations) in different forms.

– Glaze

Solves all the SWIM equations for temperatures below, at and above freezing and thus is the

most general model as it solves for the  states of water (liquid, solid and gas). It is the default

model of the Ice simulation component.

– Water film

Solves the SWIM equations for temperatures above the freezing point. Thus, no droplets/crystals

are expected to contribute to ice formation. This option is useful for solving surface water flow

problems.

– Rime

Solves the SWIM equations for temperatures well below the freezing point. In this case, all droplets

are assumed to freeze on impact and thus no runback is modeled. The energy equation is not

solved and the wall temperature remains at the recovery temperature.

Beading

When enabled, the beading model calculates variable surface roughness evolution on iced walls.

The resultant roughness is expressed as equivalent sand-grain roughness. During a multishot sim-

ulation this sand-grain roughness affects the convective heat fluxes and thus the local cooling effects

over iced surfaces. Most importantly, it eliminates the guess work of choosing an initial wall

roughness which would be applied to the entire wall uniformly. It is therefore recommended to

activate this model to obtain accurate multishot results.

Crystals

Bouncing appears in the Properties of Ice window if Crystals has been selected in the Properties

of Particles window. Bouncing enables the contribution of crystals to the icing calculation, otherwise,

Ice assumes that all crystals bounce off the surface, No bouncing. Two bouncing models are available.

NTI Bouncing Model

This model determines the amount of crystals that stick based on local surface conditions, such as

impact velocity, crystal size and film height. The model also includes an optional feature to account

for crystal Erosion effects on ice accreting surfaces.

NRC Bouncing Model

This model calculates the sticking faction based on the LWC to TWC ratio hitting the surface.

Ice density type

Four ways to specify the ice density (Constant, Macklin, Jones Glaze and Jones Rime) are supported

in Fluent Icing. By default, a constant value of  kg/m3 is set. This value has been used in many

ice shape validation cases and it is thus recommended to use this option and this value. The other

density types are correlations that uses the local ice surface temperature and other icing conditions.

For more information regarding these ice density correlations, consult Ice Density.

... Boundary Conditions

Partial differential equations are solved for each Fluent Icing component. Therefore, each component

requires a set of suitable boundary conditions. The options shown in each boundary condition type

reflect the simulation type, conditions and physical models selected/enabled in Airflow, Particles and

Ice.

Note

Fluent Icing does not offer the option to modify boundary condition types and thus they

must be set-up beforehand in Fluent.

Only a couple of Fluent boundary condition types are currently supported by Fluent Icing.

Inlet Type

– Pressure -far-field

– Velocity Inlet

– Mass-flow Inlet

– Pressure Inlet

Walls

Outlet Type

– Pressure Outlet

Symmetry

Periodic

In the next sections, a brief description of the content of Inlet, Outlet and Wall Types is provided.

Symmetry and periodic types do not require a specific set-up for icing applications and therefore are

not describe here.

.... Inlet Types

Ice accretion simulations require inlet airflow and particles boundary conditions. Four types of Fluent

boundary condition types are supported to simulate the Airflow component of Fluent Icing. Since

the Particles component only supports Dirichlet boundary conditions, particle concentration and ve-

locity conditions are specified on all Fluent boundary types.

The following figures show the Properties of each Inlet boundary type supported by Fluent Icing

when all particles type are enabled.

Airflow

To ease the set-up of the Airflow solver, it is possible to automatically define the boundary conditions

for all the Inlet types by selecting one of the two options under Conditions.

Case settings

With this option, inlet boundary conditions are automatically taken from your case file. Therefore,

this is only available if a case file has been setup beforehand with Fluent.

Edit

Edit

With this option, you can define boundary conditions that are different than those contained in

the original case file or in the Properties of Airflow settings.

The following tables map the Fluent Icing airflow boundary conditions to Fluent and FENSAP airflow

boundary conditions when Edit is selected.

Table . : Pressure Far-Field, Mapping of Airflow Fluent Icing Boundary Condition into Fluent

& FENSAP Boundary Conditions

FENSAP

Fluent

Type: Supersonic or

Far-field

Type:

Pressure-far-field

Type: Pressure-far-field

Temperature (k)

Temperature [K]

FENSAP

Fluent

Pressure

(pascal)

Gauge Pressure [Pa]

Velocity mode

---------

---------

Speed [m/s]

---------

---------

Direction mode

---------

Vector

Velocity X

X-Component of

Flow direction

X

Velocity Y

Y-Component of

Y

Velocity Z

Z-Component of

Z

Vector Angle

---------

---------

Alpha (X-Y)

[deg]

---------

---------

Beta (X-Z)

[deg]

Table . : Velocity Inlet, Mapping of Airflow Fluent Icing Boundary Condition into Fluent &

FENSAP Boundary Conditions

FENSAP

Fluent

Type:

Subsonic

Type: Velocity Inlet

---------

Supersonic / Initial Gauge Pressure

(pascal)

Velocity Mode

---------

Velocity Magnitude (m/s)

---------

---------

---------

---------

(pascal)

---------

---------

---------

---------

Normal to the boundary

Direction

Vector Components

Velocity X

X

Velocity Y

Y

Velocity Z

Z

FENSAP

Fluent

---------

---------

[deg]

---------

---------

Beta (X-Z)

[deg]

Table . : Mass Flow Inlet, Mapping of Airflow Fluent Icing Boundary Condition into Fluent &

FENSAP

Fluent

Type: Mass Flow

Type: Mass Flow Inlet

Static

Total Temperature (k)

--------

(pascal)

--------

---------

Mass Flow

Mass Flow Rate (kg/s)

Mass Flow

[kg/s]

Alpha & Beta

X

Y

Z

Normal to Boundary

--------

Mass Flow

[kg/s]

Table . : Pressure Inlet, Mapping of Airflow Fluent Icing Boundary Condition Into Fluent

Fluent

Type: Pressure Inlet

Supersonic / Initial Gauge Pressure (pascal)

X

Y

Fluent

X

Y

Fluent

Z

Note

Velocity Mode allows the use of Speed [m/s] or Mach number as a boundary condition

when the Inlet is a Pressure Far-Field or a Velocity Inlet.

Normal to the boundary defines the flow direction using the normal vectors of the

boundary surface. If selected, the Direction options do not appear. This option only appears

when the Inlet is a Velocity Inlet.

Direction allows the specification of three types of flow direction at the inlet of a Pressure

Far Field and Velocity Inlet.

If selected, the orientation of the inlet flow is defined by the following unit vector

components, Flow direction X, Flow direction Y and Flow direction Z.

If selected, the orientation of the inlet flow is defined by the following angles, Alpha

(X-Y) [deg] and Beta (X-Z) [deg].

If selected, the orientation of the inlet flow is defined by the orientation used in the

case file.

Direction mode allows the definition of two types of flow direction at the inlet of a Mass

Flow Inlet.

If selected, the orientation of the inlet flow is defined by the following normalized flow

If selected, the orientation of the inlet flow is defined by the normal vectors of the

boundary surface.

Italic Fluent and FENSAP boundary conditions shown in the mapping tables highlight conditions that

do not have a perfect counterpart in Fluent Icing.

Fluent

– X/Y/Z-Component of Flow Direction

Fluent

The Flow orientation in Fluent can be defined by a non-unitary vector. However, when using

Fluent Icing, this orientation must be provided as a normalized vector.

– Total Temperature (k)

When using Fluent as the Airflow solver in Fluent Icing, write the total temperature of a mass

flow or pressure inlet boundary condition type inside Temperature.

FENSAP

– Pressure

Static pressure is not supported by Fluent Icing. For FENSAP users, compute the Gauge pressure

by subtracting the Operating Pressure from the Static Pressure.

– Alpha and Beta angles

These angles are not supported by Fluent Icing. In FENSAP, Alpha is the angle in the X-Y plane

and Beta is the angle in the X-Z plane. Transform these angles to normalized vector components

and impose them as boundary conditions inside Direction mode → Direction Vector.

Currently, the user interface of Fluent Icing does not support turbulence boundary conditions. To

impose these conditions when using

Fluent as the Airflow solver, set them inside the original case file or modify them via the Fluent session

that is linked to Fluent Icing.

FENSAP as the Airflow solver, default turbulence boundary conditions are imposed.

– SA

Eddy/laminar viscosity ratio of 1e-

– kw-SST

Eddy/laminar viscosity ratio of  and Turbulence intensity of ..

To change these default values, use the text commands [Link to Appendix text commands] in the

Fluent Console window. For instance, to change the Eddy/laminar viscosity ratio to 1e- and the

turbulence intensity to 1e-, type the following commands:

– /icing/settings/set flow/turb_eddy_lam_ratio 1e-

– /icing/settings/set flow/turb_intensity 1e-

A zero value to these settings will revert them to their default value. Such text commands can also

be sent from Fluent Icing by using the Send Command action, in the contextual menu of the case

file.

Note

To learn more about these Fluent Inlet boundary conditions, consult Pressure Far-Field

Boundary Conditions, Velocity Inlet Boundary Conditions, Mass-Flow Inlet Boundary Condi-

tions and Pressure Inlet Boundary Conditions within the Fluent User's Guide. To learn more

about FENSAP Inlet boundary conditions supported in Fluent Icing, consult Inlets and Far-

fields – -BCs.

Particles

To ease the set-up of the Particles solver, it is possible to automatically define the boundary conditions

at the Inlet by checking Automatic. In this case, the Properties of Particles settings are applied as

boundary conditions and it is assumed that particles and airflow share the same inlet velocity.

The following lists the boundary conditions of all types of Particles when the Automatic option is

unchecked.

• Droplet Boundary Conditions

Droplet boundary conditions are available if Droplets has been selected in Set-up → Particles

– Droplet LWC [kg/m3]

Set the water droplet concentration at the Inlet.

– Droplet diameter

Set the MVD of the spherical particle that represents a cloud of water droplets at the Inlet. This

option is available when the Break-up model has been activated inside Set-up → Particles →

Droplets

– Droplet temperature [K]

Droplets

Set the temperature of the cloud of water droplets at the inlet. This option is available when the

Particle thermal equation is enabled in Set-up → Particles.

– Droplet custom velocity

When enabled, this option allows the specification of an inlet droplet velocity that is different

than the airflow velocity at the inlet. In this case, set the velocity components (Droplet X velocity

[m/s], Droplet Y velocity [m/s], Droplet Z velocity [m/s]) of the water droplet cloud.

Crystal Boundary Conditions

Crystal boundary conditions are available if Crystals has been selected in Set-up → Particles.

– Crystal ICC [kg/m3]

Set the ice crystal concentration at the Inlet.

– Crystal temperature [K]

Set the temperature of the cloud of ice crystals at the inlet. This option is available when

the Particle thermal equation is enabled in Set-up → Particles

– Crystal custom velocity

When enabled, this option allows the specification of an inlet ice crystal velocity that is different

than the airflow velocity at the inlet. In this case, set the velocity components (Crystal X velocity

[m/s], Crystal Y velocity [m/s], Crystal Z velocity [m/s]) of the ice crystal cloud.

Vapor Boundary Conditions

Vapor boundary conditions are available if Vapor has been selected in Set-up → Particles

– Condition mode

Set the type of vapor boundary condition to impose at the inlet.

– → Relative Humidity [%]

Set the relative humidity at the inlet. This value is defined as the ratio of partial vapor pressure

to the saturation vapor pressure.

→ Vapor Concentration [kg/m3]

Set the vapor concentration at the inlet.

Note

Note

In the case of Inlet boundaries that share inlet and outlet cells, the Particles solver will

identify the cells that are inlets based on the velocity components of droplets and crystals

that have been specified under Particles.

Built-in Inlet type commands are available by right-clicking the inlet type icon in the Outline View.

Two commands are currently supported.

Copy from Airflow settings

Copies the Properties of Airflow settings into the Airflow submenu of the Properties of the

Inlet window when Edit is selected in Conditions.

Display

Displays the surface mesh of the Inlet type selected in the Graphics window.

....Wall

Ice accretion simulations require appropriate airflow, vapor and icing wall boundary conditions. The

following figure shows the Properties of each Wall boundary type supported by Fluent Icing.

Airflow

In the current version of Fluent Icing, all walls are stationary with No slip condition unless otherwise

specified in the original case file. The No slip condition will allow the natural growth of the viscous

layer, crucial for icing calculations.

The following table maps the Fluent Icing airflow wall boundary conditions to Fluent wall boundary

Mapping of Airflow Fluent Icing Wall Boundary Conditions into Fluent & FENSAP Boundary

Conditions.

FENSAP

Fluent

---------

Heat Flux

Heat Flux (w/m2)

Heat Flux [W/m2]

---------

Sand-grain

roughness

High Roughness (Icing) / Specified

Roughness

High roughness for Icing

Heat Flux

---------

roughness

Roughness

Thermal Conditions allows the specification of three types of energy equation boundary conditions

at the wall.

If selected, specify a temperature at the wall. For ice accretion simulations over a wall, set a tem-

perature that is equal t o the adiabatic stagnation temperature + 10K. This temperature is used to

compute convective heat transfer coefficients in the Ice component. Thus, the Ice component will

provide the real temperature profile over the wall.

If selected, specify a heat flux at the wall. If all walls of your computational domain are set to

adiabatic conditions (zero heat flux), Fluent Icing will automatically activate EID. EID is a feature

that improves the accuracy of icing calculations for high Mach number flows, important to accurately

predict beak ice phenomenon. For more information regarding this model, consult Extended Icing

Data (EID)

If selected, the thermal condition specified in the Fluent case file is used. For more information,

consult Thermal Boundary Conditions at Walls within the Fluent User's Guide.

Wall Roughness allows to specify two types of roughness properties at the wall.

High Roughness for Icing

If selected, specify a Roughness Height (m) at the wall. By default, Fluent Icing sets a Roughness

Constant of . in Fluent. This value describes a uniform sand-grain roughness distribution. In

FENSAP, the Roughness height (m) parameter always applies a constant roughness distribution

and therefore the Roughness Constant parameter is not required. For ice accretion simulations

over a specific wall, it is recommended to set the roughness height to . m, a value extensively

used during validation exercises. When running a multishot calculation, this value will either be

replaced by the roughness distribution computed by the beading model at the previous shot, if

selected in Set-up → Ice, or remain constant during the entire multishot calculation. For more in-

formation regarding the High Roughness model, consult Additional Roughness Models for Icing

Simulations (p. ).

If selected, the wall roughness condition specified in the Fluent case file is used. For more inform-

ation, consult Setting the Roughness Parameters (p. ).

Particles

Among all Particles type, only the vapor model provides a wall boundary condition option that allows

the walls to stay at % relative humidity and enables evaporation at these walls. To set this

boundary condition check the Vapor Wet wall condition.

Ice

Ice is computed over the walls of the computational domain. Two options are provided under ice,

the first (Icing) enables or disables walls from participating in solving the PDEs of the Shallow Water

Icing Model (SWIM), thus reducing computational time when walls are disabled, the other (Specify

Heat Flux) allows setting a heat flux on a wall to examine its impact on the ice accretion process.

The latter could be used to quickly assess the amount of heat required to prevent ice formation, for

instance.

Icing, just under Ice, is divided into five options:

instance.

Enabled

This is the default setting under Icing and it allows this wall to be part of the computational domain

of SWIM.

Disabled

If selected, it will remove this wall from the computational domain of SWIM.

Enabled - Sliding

If selected, it will allow the wall to take part of the computational domain of SWIM, but no ice will

be allowed to accrete over this wall. The wall will act as a sliding surface for adjoining surfaces,

that can accrete ice, to slide on.

Disabled - Sliding

If selected, it will remove this wall from the computational domain of SWIM. However, the wall will

act as a sliding surface for adjoining surfaces, that can accrete ice, to slide on.

Sink

If selected, liquid water film will not be allowed to enter this wall and this wall will act as an exit.

Built-in wall commands are available by right-clicking the Wall icon in the Outline View. Two com-

mands are currently supported.

Set Temperature to Adiabatic+

Sets a temperature to the wall that is equal to the adiabatic stagnation temperature, using the

Properties of Airflow settings, plus  K. In this manner, inside the Airflow submenu of the

Properties of the wall window, the Thermal Conditions will automatically switch to Temperature

and the appropriate temperature will be shown next to Temperature [K].

Display

Displays the surface mesh of the wall selected in the Graphics window.

.... Outlet Types

One outlet type is currently supported by Fluent Icing. It is the Pressure Outlet.

Only one field can be modified through the Properties window of that boundary condition. It is the

Gauge Pressure [Pa] and it corresponds to the Gauge Pressure (pascal) in Fluent. The Gauge Pressure

is the result of subtracting the Operating Pressure from the Static Pressure variable used in FENSAP

to specify a Subsonic outlet.

Note

If more Pressure Outlet settings are required, for instance more settings could be needed

in order to define flow reversal conditions at the outlet, add them inside the original case

file or through the Fluent session connected to Fluent Icing.

... Solve

In Solve, you will define the solver settings of your Fluent Icing simulation including monitoring, ini-

tialization and output files for each of its Fluent Icing components (Airflow, Particles and Ice). These

solver settings will allow you to conduct the five simulation scenarios mentioned in Set-up (p. ) as

long as they have been properly selected in the Properties of Set-up window.

The Properties of Solve window provides the multishot and general settings for all Fluent Icing

components.

Multi-shot

The Multi-shot menu in Properties of Solve is only available when all three solver types have been

selected in the Properties of Set-up. See Multi-Shot (p. ).

This submenu sets the common output and monitoring settings of all Fluent Icing components.

– Plot update interval

Controls the frequency of residual output and variables that are monitored. A value of  disables

all plotting.

– Auto-save solutions

Automatically saves the solution of each Fluent Icing component.

– Log verbosity

Controls the amount of convergence and execution information displayed (Minimal, Complete,

Detailed) inside the Console window. Its content varies for each Fluent Icing component.

– Save convergence to file

Writes convergence files for each Fluent Icing component inside your working directory

→ *.fconverg for the Airflow component when using FENSAP.

→ *.iconverg for the Ice component

These convergence files contain the history of your residuals.

Fluent Icing components shown under Solve in the Outline View window are accompanied by an

icon to their left. This icon reports if a solution file has been loaded or computed. The following table

shows these icons.

Ice

Particles

Airflow

Solution not loaded or

computed

Solution loaded or

computed

To run a multishot calculation, first complete the set-up of all the Fluent Icing components under

Solve, then right-click the Solve icon in the Outline View and select Run multishot.

The Properties of Airflow window under Solve permits the configuration of the airflow solver,

monitor and output parameters. Depending on the Airflow solver selected in Set-up, the Properties

of Airflow window will show either Fluent or FENSAP parameters. Only steady-state airflow simulations

are supported in Fluent Icing.

Fluent Properties of Airflow Window

Only the Number of iterations to run a steady calculation is supported in this window. Other Fluent

Solution UI parameters, such as Methods, Controls, Monitors, Initialization, etc., must already be

present in the original case file or modified via the Fluent session linked to Fluent Icing.

The Results - Fluent submenu shows that a data file has been loaded or computed when Loaded

is checked.

An additional option is available in this window when an Ice solution with beads has been previously

run and loaded to your Fluent Icing simulation. It is the Roughness from beading.

By enabling this option, the roughness distribution computed by the beads model will be applied as

a boundary profile on all walls where the High roughness – Icing model has been enabled. The

Roughness Height (m) of these walls will be updated to ICE3D Roughness file, which uses the

ROUGHNESS boundary profile, the sand-grain beads profile, computed by Ice.

FENSAP Properties of Airflow Window

The Properties of Airflow window contains the most common steady-state solver and monitoring

settings of the FENSAP airflow solver.

The Time integration (FENSAP) submenu allows the set-up of the pseudo time step number, CFL,

as well as the Number of iterations to use during the simulation. If convergence problems are en-

countered, reduce the CFL or activate the CFL ramping iterations option and specify a number of

CFL ramping iterations. This option gives access to a mechanism that linearly increases the CFL

number from , at the start of the simulation, to its full value at the end of the CFL ramping iterations.

The Output submenu allows the creation of numbered solution files and of the most common

monitoring variables to track in order to guarantee full convergence of the FENSAP solver.

Forces

Forces

By default, No lift and drag coefficients are outputted during the simulation. However, if Forces

is set to Drag-Custom direction, resultant lift, drag and moment coefficients (on all walls) will be

monitored during the simulation. These aerodynamic coefficients are computed using the Conditions

defined in Set-up → Airflow and the following parameters.

– Lift axis

Provide the positive orientation of lift along the positive or negative X, Y and Z axis. FENSAP will

obtain its true direction based on this information and the drag direction.

– Drag – X, Drag – Y, Drag – Z

Provide the non-dimensional direction of drag in Cartesian coordinates.

– Reference area

Specify a reference area in m2 that is used to compute the aerodynamic coefficients.

– Moment – X, Moment – Y, Moment – Z

Specify a point in the computational domain that will act as the moment center to compute the

aerodynamic moment coefficient.

Numbered solution files

If selected, specify the frequency, Iterations between output, at which FENSAP solutions are going

to be written inside your working directory. This option does not overwrite solution files and

therefore an iteration number will be assigned as a suffix to the airflow solution file name. Make

sure that you have enough disk space when you select this option.

Monitor - Total Heat

If selected, monitors the total convective heat flux using all the walls of the computational domain.

Monitor -Mass Flow

If selected, monitors the mass inflow, outflow and deficit of air inside the computational domain.

Monitor -Heat Flux

If selected, monitors the total enthalpy inflow, outflow and deficit of the computational domain.

ROUGHNESS boundary profile, sand-grain beads profile computed by Ice.

Airflow Commands

Built-in airflow commands are available by right-clicking the Airflow icon under Solve in the Outline

View. The following commands are currently supported.

Executes an initialization of the airflow solver using the Initialization settings of Fluent or in the

case of FENSAP, the Conditions and Direction parameters in Set-up → Airflow.

Calculate

Launches the simulation of the Airflow component. If a solution is loaded, the simulation will

continue from that loaded solution. Otherwise, Calculate will first Initialize and then use this

solution to solve the PDEs of the Airflow component.

Interrupt

Stops the execution of the airflow solver at the end of the next iteration. The solution is kept in

memory.

Load/Save/Save as…

Load or save files into or from your Airflow simulation.

The Properties of Particles window contains the most common steady-state solver, initialization and

monitoring settings of the Fluent Icing Particles solver, DROP3D.

The Run settings submenu allows the set-up of the Number of iterations to conduct during the it-

erative simulation.

The Solver submenu is divided into three points, the pseudo time step, the artificial viscosity and

the convergence criteria.

CFL

The recommended values for the CFL range between  and . If convergence problems are encountered,

reducing the CFL might help.

Artificial Viscosity coef

The Particles component uses the Streamline upwind (SU) technique to stabilize the PDEs. This

scheme is complemented with a user-set crosswind diffusion. Its default value is 1e- and has been

extensively used in a large number of validation cases. In the case of structured grids, you can in-

crease this value to 1e- if you experience oscillations of LWC within the shadow zone. Its impact

to collection efficiency is generally minimal. Crosswind dissipation scales with mesh size, similar to

the upwind scheme, and is lower with finer grids.

Residual cut-off

The Residual cut-off is the stopping criterion of the overall residual of the Particles governing

equations. Lower the default value of 1e-, especially if you are interested in capturing shadow

zones.

Change in total beta

This parameter is the difference in total collection efficiency of all walls between two consecutive

iterations. It is thus a measure of convergence of the number of particles (droplets or crystals) that

hit the walls of the computational domain. Lower the default value of 1e- if you see differences

in collection efficiency between printouts.

The Initialization submenu allows the initialization of the particle concentration and particle velocity

fields.

Velocity

Two initialization choices are offered for the velocity field.

– From Airflow conditions

If selected, the Speed and Direction inside of Set-up → Airflow are used as the initial velocity

of all types of particles at all nodes in the computational domain.

– Cartesian components

If selected, specify the velocity components (X velocity [m/s], Y velocity [m/s] and Z velocity

[m/s]) that will be assigned as the initial velocity for all particles inside the computational domain.

Dry Initialization

If selected, sets the particle concentration (LWC, ICC or Vapor Humidity) to zero everywhere inside

the computational domain except at the inlet, where Particles boundary conditions are defined.

Otherwise, the Particles concentration specified in Set-up → Particles will be used to initialize the

computational domain.

The Output submenu contains two options:

Numbered solution files and Save distribution solutions.

If selected, specify the frequency, Iterations between output, at which Particles solutions written

inside your working directory. This option does not overwrite solution files and thus an iteration

number will be assigned as a suffix to the Particles solution file name. Make sure that you have

enough disk space when you select this option.

Save distribution solutions

Select this option if you would like to save all the solutions of a distribution simulation. The solutions

will be numbered from  to the total number of particles sizes that define this distribution. The

number  will be assigned to the largest particle size and the last number to the smallest particle

size.

The Monitors submenu allows the tracking of convergence of surface integral quantities such as

collection efficiency, mass deficit and vapor condensation.

Total Beta

– If selected, monitors the total collection efficiency computed on all walls of the computational domain.

Change in Total Beta

– If selected, monitors the difference in total collection efficiency of all walls between two consecutive

Mass deficit

– If selected, monitors the mass inflow, outflow and deficit of particles inside the computational domain.

Vapor condensation

– If selected, monitors the total vapor condensation on all the walls of the computational domain.

Note

In a particle distribution simulation, each particle size simulation is executed in sequence.

Their residuals graph is displayed at the end of the execution and will present a summary

of the convergence of each calculation.

Particles Commands

Built-in particles commands are available by right-clicking the Particles icon under Solve in the

Outline View. The following commands are currently supported.

Executes an initialization of the Particles solver using the Initialization settings inside the Solve →

Particles property window.

Calculate

Launches the simulation of the Particles component. If a solution is loaded, the simulation will

Calculate

continue from that loaded solution. Otherwise, Calculate will first Initialize and then use this initial

solution to start solving the PDEs of the Particles component.

Load

Load a Particles solution to your Fluent Icing simulation.

Save Droplets

Saves only the water droplet solution files of your Particles simulation. The name of this file will

be your case filename (without the .cas suffix) followed by .droplet.

Save Crystals

Saves only the ice crystal solution file of your Particles simulation. The name of this file will be

your case filename (without the .cas suffix) followed by .crystal.

Save Vapor

Saves only the vapor solution file of your Particles simulation. The name of this file will be your

case filename (without the .cas suffix) followed by .vapor.

Reset

Unloads the Particles solutions.

.... Ice

The Properties of Ice window contains the most common time, initialization and output settings of

the Ice solver, ICE3D.

The Time submenu allows the set-up of the Total time of ice accretion [s] and the type of time step.

Total time of ice accretion [s]

This is the total physical time duration of the Ice simulation.

Automatic time step

By default, this option is checked. The stable time step for an explicit time integration scheme de-

pends on fluid speed and local mesh sizing. For time accurate problems, all control volumes have

to use the same time step. Automatic time stepping removes the guess work of specifying a stable

time step. In this manner, this option computes the optimal time step for each grid/film speed

combination and largely reduces your computational time. If disabled, a Time step [s] option ap-

pears, where you can define a stable time step for the Ice simulation.

The Initialization submenu allows the continuation of a simulation from an existing ice solution. If

an ice solution has been loaded or obtained, the Restart from current solution becomes available

and, if selected, the Ice simulation will use the loaded or obtained solution as a starting point of the

unsteady ice calculation.

Note

By default, Calculate will run the Ice simulation without considering loaded files as initial

solutions. To start the calculation from a given solution, you must initialize your simulation

by using Restart from current solution.

The Output submenu allows the selection of the type of Ice simulation to conduct.

Run icing

Runs the SWIM as well as the ice shape model and therefore produces an ice solution. This option

is checked (enabled) by default.

Run grid displacement

If selected, this option will output a 3D grid displaced by the accumulated ice on the solid

boundaries. Therefore, this option requires an ice solution. When selected with Run icing, the Run

icing is executed first and then the Run grid displacement follows. When Run grid displacement

is the only option selected in Output, an ice solution must be loaded.

Note

In a multi-shot simulation, Run icing and Run grid displacement are automatically executed

in sequence.

After grid displacement, the walls and the surrounding cells are displaced/deformed to

Note

take into account the new ice shape. The next step in this process would be to run the

airflow solver on this new grid in order to obtain the local airflow conditions and properties

around the new ice shape. Further calculations (particles and ice) are obtained on the up-

dated mesh. Therefore, each shot has its own grid/case file.

The Result submenu appears if an ice solution has been Loaded (loaded or calculated). This is also

displayed in the Outline View window by the icon

next to Solve → Ice.

Ice Commands

Built-in ice commands are available by right-clicking the Ice icon under Solve in the Outline View.

The following commands are currently supported.

Calculate

Launches the simulation of the Ice component based on the settings defined in Solve → Ice.

Load

Loads an Ice solution to your Fluent Icing simulation. To use this solution as a restart, enable Restart

from current solution inside the properties window of Solve → Ice.

Save

Saves all Ice solution files of your simulation. The name of these files will be your case filename

(without the .cas suffix) followed by .ice.*. The suffixes * are ice.grid, map.grid and

swimsol. For more information regarding these output files, consult Results (p. ).

Reset

Unloads the Ice solution.

.... Multi-Shot

A multi-shot run executes the three solvers (Airflow, Particles, Ice) in sequence.

This option allows the control of the number of quasi-steady shots,Number of shots, to simulate and

the saving of output files of Airflow, Particles and Ice at each shot, Save files at each shot, for future

post-processing if needed.

Number of shots

This option allows the control of the number of quasi-steady shots to simulate, which is one instance

of Airflow – Particles – Ice calculation. Grid displacement is executed at the end of each shot and

used as an input for the next step.

Save files at each shot

The solution of each solver step will be saved in separate files on the disk, alongside the case file.

The files are numbered for each shot, for example casefilename..droplet is the droplet

solution for shot #.

Multi-Shot Commands

Built-in multi-shot commands are available by right-clicking the Solve icon in the Outline View. The

following commands are currently supported.

Run multishot

Executes the multi-shot sequence for Number of shots. The current state of the execution (solver

and shot step) is displayed in the Outline View. The grid file is displaced with the ice shape at the

end of each shot.

Interrupt

Stops the multi-shot computation at the current step. The solution is saved at the current state.

This is available when the multi-shot simulation is running.

Reset

Resets and unloads all solutions. This is equivalent to executing Reset on each Airflow, Particles

and Ice tree nodes. The grid file is not reset by this operation. If the Airflow solver is Fluent, Reset

will execute an initialize operation on the airflow solution.

Note

The multi-shot morphs the grid with the iced wall surfaces at each shot. The Reset op-

Note

eration will reset solutions, but will not load the original grid node locations. To revert

to a specific shot, or the original grid, use the File → Open menu and select the appro-

priate case file to load. Loading a case file will also load its settings in Fluent Icing.

A multi-shot sequence can be manually set by executing the Airflow, Particles, Ice

solvers one after the other. In this case, enable Run grid displacement in Solve → Ice

to account for ice shape updates within the 3D grid and, if the Beading model is used,

active Roughness from beading in Solve → Airflow to consider the impact of the sand-

grain roughness produced by the beads onto the airflow.

... Results

The Results section in the Outline View provides access to the core Fluent postprocessing options

as presented in the Remote Visualization Client and offers the same options as in Fluent’s user interface.

The different object types offered under Result → Graphics are:

Meshes

Displays the current mesh surfaces.

Contours

Displays contours of solution fields over surfaces. The results of Fluent Icing are listed in the Icing

variable category. The list of available Fluent Icing fields will depend on the solution files currently

loaded (airflow, droplets, crystals, vapor, ice). All Fluent Icing fields are solutions defined at the nodes.

Vectors

Displays vector solution fields in the entire computational domain or on selected surfaces. Only

supported for Fluent airflow solution variables. Use Viewmerical or CFD-Post to post-process FENSAP,

Particles and Ice vector solutions.

Pathlines

Pathlines

Displays flow and particle paths within the computational domain. Only supported for Fluent airflow

solution variables. Use Viewmerical or CFD-Post to post-process Particles and Ice pathlines.

Some mesh and common Fluent Icing fields can be viewed quickly by using Quick-view. See the next

section for more details.

To create and display a new graphic object:

Right-click on the object type of interest (Meshes, Contours, etc. ), and select New

or use the command buttons in the View window of the Ribbon.

In the Property window, set-up the graphical object options, and choose the Surfaces to display. A de-

scription on how to generate these object types can be found inside Basic Graphics Generation of the

Fluent User's Guide.

Select Display in the contextual menu of the new object to output the result in the Graphics window.

.... Quick-View

Quick-view permits to easily output the most common Fluent Icing fields on walls and other boundary

surfaces. A Fit to Window view is applied in all cases by default.

Note

Quick-view will use the solution data of the currently selected Fluent case file. To output

the solution of another Fluent case within the Outline View, select the desired case before

running Quick-view.

Three object types are supported in Quick-view.

Mesh

All boundaries

Displays the boundary surface meshes of computational domain (inlet, outlet, wall, symmetry)

Walls only

Only the wall surfaces are displayed.

Mesh – Viewmerical

Opens Viewmerical with the mesh of the simulation case.

Mesh – CFD-Post

Walls only

Opens CFD-Post with the mesh of the simulation case.

Contours

Airflow

– FENSAP/Fluent

–

Temperature (walls)

→

Displays the temperature distribution on all walls.

→ Heat flux (walls)

Displays the convective heat flux distribution on all walls.

→ Velocity Magnitude

Displays the airflow speed on all boundary surfaces.

– FENSAP format only

→ View with Viewmerical

Opens Viewmerical with the mesh and the airflow solution of the simulation case.

→ View with CFD-Post

Opens CFD-Post with the mesh and the airflow solution of the simulation case.

Particles

– Droplets / Crystals

→ Collection efficiency

Displays the collection efficiency of the droplets or crystals on all walls.

→ LWC / ICC

Displays the LWC or ICC on all boundary surfaces.

Opens Viewmerical with the mesh and the droplet or crystal solution of the simulation case.

Opens CFD-Post with the mesh and the droplet or crystal solution of the simulation case.

Vapor

– Vapor concentration

Displays vapor concentration on all boundary surfaces.

– Vapor condensation

Displays vapor condensation on all walls.

– View with Viewmerical

Opens Viewmerical with the mesh and the vapor solution of the simulation case.

– View with CFD-Post

Opens CFD-Post with the mesh and the vapor solution of the simulation case.

Ice

– Ice thickness

Displays the ice thickness on all walls.

Opens Viewmerical with the surface mesh (map.grid) and the ice solution (swimsol) of the

simulation case.

Opens CFD-Post with the surface mesh (map.grid) and the ice solution (swimsol) of the

Ice cover

Ice cover

Viewmerical / CFD-Post

Displays the 3D ice shape over the original surface. In the case of CFD-Post, the display of the ice

shape is done by executing the Ice Cover – 3D-View icing macro.

Multishot ice cover

Displays the 3D ice shapes obtained during each shot over the original surface. In the case of CFD-

Post, the display of all ice shapes is done by executing the Ice Cover – 3D-View icing macro.

A single quick-view item can be displayed at a time in the Graphics window and will replace the

previous item displayed. To store multiple items in different windows, use the Results entry in the

Outline View as detailed in Results (p. ).

Selecting a quick-view will reset the current view. To update the current quick view with the latest

solution, use the Display command from the contextual menu in the Outline View.

For more information regarding Viewmerical and CFD-Post, consult the next two sections.

....Viewmerical

Viewmerical is the post-processor of FENSAP-ICE and can read icing solutions directly. Usage is detailed

in Viewmerical.

Viewmerical will read a grid and solution file in FENSAP format. When using the Quick-view Viewmer-

ical commands, temporary files (*.TMP files) are written and Viewmerical is launched with these files.

For example, a case file, CASE.cas, was used to obtain an airflow and water droplet solutions. If you

decide to open the water droplet solution with Viewmerical within Quick-view, the following temporary

files are written

CASE.tmp.grid

This is the temporary FENSAP grid file.

CASE.tmp.droplet

This is the temporary droplet solution file.

These temporary files can be deleted without compromising your Fluent Icing simulation workflow.

Note

Launching Viewmerical requires a Post-processing license token and the installation of the

FENSAP-ICE package. FENSAP-ICE is part of the default Fluids installation package of ANSYS.

Launching it requires the AWP_ROOT*** environment variable to be set-up. This is auto-

matically done on Windows during the installation process. See the ANSYS installation

manual for details

.... CFD-Post

CFD-Post is a general post-processor for ANSYS Fluids and can read icing solutions directly via a

command file. Usage is detailed in the CFD-Post section of the CFX-Pre User's Guide.

CFD-Post is launched with special icing macros enabling the generation of figures and animations of

ice shapes and field contours in 3D (Ice Cover – 3D-View) as well as 2D Plots (Ice Cover – 2D-Plot),

their usage is detailed in the CFD-Post Macros section within the FENSAP-ICE User Manual.

CFD-Post will read a grid and solution file in FENSAP format as well as a command file. When using

the Quick-view CFD-Post commands, temporary files (*.TMP files) are written and CFD-Post is launched

with these files.

For instance, a case file, CASE.cas, was used to obtain an airflow and water droplet solutions. If you

decide to open the water droplet solution with CFD-Post within Quick-view, the following temporary

files are written:

Case.tmp.fsp

This the temporary command file.

Note

CFD-Post is installed by default with any ANSYS Fluids product and uses a Post-processing

license token. Launching it requires the AWP_ROOT*** environment variable to be set-

up, this is automatic on Windows as the software is installed. See ANSYS, Inc. Installation

Guides for more details.

... Preferences

The Icing preferences are available from the File → Preferences menu.

Fluent Icing launch options are set-up in this window:

Launches a Fluent session when opening Fluent Icing.

Default Fluent CPU

Specifies the number of CPUs used during Fluent Icing simulations.

Define working directory

If enabled, permits the definition of a working directory where case files are imported and future

simulation files are written. Its location should be defined inside the Working directory text box.

If disabled, future simulation files will be written where the original case file is located.

Enables Beta features of Icing solvers

Advanced settings

See Advanced Settings (p. )

... Advanced Settings

Some expert level options are unavailable at the start of Fluent Icing as they are rarely used during

icing simulations. These options should be used with cautious. When the Advanced settings option

is enabled in Preferences, the following extra options appear in Fluent Icing.

Turbulence Schmidt number

Appears in Set-up → Particles → Vapor. The Turbulent Schmidt number is proportional to the

turbulent mass diffusion coefficient of the vapor transport equation. Therefore, it controls the rate

of propagation of water vapor. Its default number is set to . and has been used in several validation

cases.

Disable EID Preprocessing

Appears in Solve → Ice. In some scenarios related to Adiabatic walls (see Boundary Conditions (p. ),

Inlet Types (p. ), Airflow (p. ) and Heat Flux under Ice (p. )), the EID pre-processing will be

executed, prior to executing the Ice solver. If this option is enabled, the EID preprocessing will be

skipped. If the EID was already computed onto the current airflow, the Ice simulation will use the

existing EID solution. If EID was not computed onto the current airflow, the Ice simulation will use

the solution without the pre-processing.

Note

The EID preprocessing is mandatory for simulations incorporating vapor transport.

Save GMRES to file

Appears in Solve. This option saves an additional file, the *. *gmres file, to monitor convergence

of the GMRES solver in FENSAP and Particles.

Heat Flux

Appears in Set-up → Ice. This option allows the selection of two types of convective heat flux pro-

duced by FENSAP in order to conduct an ice accretion simulation.

– Classical

Convective heat fluxes computed using temperature gradients on the walls. This method is 2nd

order accurate and is the default option when Advanced settings is disabled.

– Gresho

Convective heat fluxes computed based on Gresho’s Consistent Galerkin formulation. Gresho

– Gresho

fluxes tend to exhibit oscillations when the surface grid is uneven or coarse and therefore it is

less robust than Classical.

... File Types

The following describes the type of files generated/loaded/imported by Fluent Icing:

Starting Input File

.cas

Fluent case file. Contains the grid and configuration of your Fluent/Fluent Icing simulation.

.cas.gz (compressed case file) and *.cas.h5 (HDF / CFF case file) can also be used.

Airflow

.dat

Fluent airflow solution file

.dat.gz and *.dat.h5 are used, if the case file is in .gz or .h5 format.

*.soln

FENSAP airflow solution file.

Particles

.droplet

Water droplet solution file.

.crystal

Ice crystal solution file.

.vapor

Vapor solution file.

Ice accretion

.swimsol

Ice solution file (can be viewed with map.grid or ice.grid).

.map.grid

Surface mesh of walls that have been enabled for icing.

.ice.grid

Surface mesh of the ice shape produced by walls that have been enabled for icing

Ice accretion – extra files.

.swimsol.s2g

Mapping file to load a swimsol (areal solution) in Fluent. Automatically loaded/saved alongside a

swimsol file. Required for Fluent Icing.

.rough

Roughness profile when beading is enabled.

.disp

Displacement profile that represents the volumetric accretion of ice.

Residuals (if Save convergence to file is enabled in Solve).

.fconverg

FENSAP airlfow convergence.

.fgmres

FENSAP airflow GMRES residuals.

.pconverg

Particles convergence.

FENSAP grid (if Write FENSAP... grid is selected under File → Export).

.grid

.fgmres

.pconverg

.grid

FENSAP grid file. This grid can be used in Viewmerical or CFD-Post to view Particles solution files.

Multishot

..*

Files related to the first shot.

..*

Files related to the second shot.

Etc.

Control files

.abort

Batch mode computation interruption file. See Interrupting a Computation under Fluent Journal

Commands (p. ).

cleanup-fluent-*.bat / cleanup-fluent-*.sh

Script file enabling a kill of the Fluent process and subprocesses. This is not required in regular exe-

cution mode.

cleanup-flicing-*.bat / cleanup-flicing-*.sh

Script file enabling a kill of the Fluent Icing process.

Temporary files – Can be safely erased after execution

fluent-*-error.log

Temporary log files for Fluent error conditions.

serverinfo. *

File used to connect Fluent Icing to the Fluent server, also generated by running File → Applications

→ Icing or File → Applications → Server → Start in Fluent main application.

.cmd.3dview*, *.3dtmp

Cache files used by Viewmerical.

.fsp

Command file used to launch CFD-Post.

.tmp. *

Temporary grid & solution files used to launch Viewmerical or CFD-Post.

... Appendix

.... Python Commands

Many of the icing features and settings can be accessed and changed through the Console window,

using python commands.

The same commands can be used to automate the Fluent Icing application, by launching it with the

R argument, as in:

Linux

bin/icing -wait -R file.py

Windows

bin/icing.bat -wait -R file.py

The -wait argument waits until the execution is completed, before resuming batch execution.

Linux

Windows

Without the -wait command, the Fluent Icing application is sent to background).

Note

The batch mode requires a graphical display. To run a case file in batch, use Fluent

Journal Commands (p. ).

Python Console & Operations

The Console window at the bottom right corner of the Fluent Icing application permits to enter

commands interactively. The following sections describe commands available in the python console

dir() and the command/attribute list

dir()

Display the list of global commands and top-level objects.

'AddSession', 'ReadScriptFile', 'RemoteSession', 'StartTranscript', 'StopTranscript'

dir(object

Display the list of commands & attributes of the object.

Example . : Entering Commands Interactively

(Assuming test1.cas is already loaded)

dir(RemoteSession[“test1.cas”])

'Case', 'Connect', 'ConnectionInfo', 'IcingSimulation', 'StartServer'

r = RemoteSession[“test1.cas”] #

A temporary variable can be used to simplify command lines.

dir(r.Case.Icing.Particles)

'Crystals', 'Droplets', 'Model', 'Type', 'Vapor'

dir(r.Case.Icing.Particles.Droplets.Particles.Droplets.Conditions)

' Appendix', 'Diameter', 'LWC', 'SLDFlag', 'WaterDensity'

Accessing/Changing values

The () operator will return the current value of the attribute.

RemoteSession[“test1.cas”].Case.Icing.Particles.Conditions.LWC()

.

RemoteSession[“test1.cas”].Case.Icing.Particles.Conditions.LWC = .

Commands

If an item listed in dir() is a verb, it is a command.

For example

AddSession()

RemoteSession[“test1.cas”].Case.Icing.Solution.ParticlesRun.Calculate()

Commands

Sample script

# Add sesssion and load case file

r = RemoteSession["RemoteSession1"]

r.IcingSimulation.Inputs.CaseFile = "grid.cas"

r.IcingSimulation.Inputs.DataFile = "grid.dat"

r.StartServer()

# Airflow: already set-up in case file (Fluent airflow)

# Droplets: Configure

r.Case.Icing.Particles.Droplets.Conditions.Diameter =

r.Case.Icing.Solution.ParticlesRun.Solver.CFL =

r.Case.Icing.Solution.ParticlesRun.RunSettings.NumIterations =

# Wait until the boundary conditions are loaded and available to set-up

waitTrue(r.Case.Icing.IcingBC)

# Setup boundary conditions

bc = r.Case.Icing.IcingBC["velocity-inlet-"]

bc.ParticlesInlet.AutoBC = False

bc.ParticlesInlet.DropletDiameter =

bc.ParticlesInlet.DropletTemperature =

bc.ParticlesInlet.DropletVelocityFlag = True

bc.ParticlesInlet.DropletVelZ = .

# Compute droplets

r.Case.Icing.Solution.ParticlesRun.Calculate()

r.Case.Icing.Solution.ParticlesRun.SaveDroplets(Filename="test1.droplet")

# This script will stop after execution.

r.Disconnect()

.... Fluent Journal Commands

Once a case is configured in the Icing application and saved, it can be used in batch mode scenarios

where a regular Fluent journal file is used.

Use regular Fluent journal file commands to execute standard Fluent operations:

Load/save the case file

Load/save the data file (.dat)

Initialize/Iterate the Fluent airflow solution

Etc.

In a case file where icing was set-up with the Fluent Icing application, the text command environment

will provide the icing/ submenu and commands:

icing/

– file/

– settings/

– flow/

– drop/

– ice/

icing/

– file/

– flow/

– drop/

– ice/

– multishot/

file/ commands

– load-file / save-file

→ Load or save a single solution file, of a specified type

– load-all / save-all

→ Load or save all solution files associated with a .cas

For FILE.cas, the default output filename is the filename without the suffix (FILE).

The command would write FILE.droplet, FILE.swimsol, etc.

– reset-file

→ Unload a specific solution type

– reset-all

→ Unload from memory all icing solutions (FENSAP airflow, particles, ice)

– status

→ List the currently loaded icing solutions, and their type

settings/

– get variable

– set variable value

→ Individual icing settings can be accessed and changed through these commands.

Advanced users: The settings are the rpvar name without the fensapice/ prefix

– auto-save?

→ Toggle the auto-save feature, which is writing solutions to files at the end of any icing solver run

(airflow, particles, ice).The file is written alongside the case file (FILE.cas will have FILE.droplet,

etc.)

– save-converg? save-gmres?

→ Toggle to save the convergence detail of icing solvers in text files alongside the case file

– verbosity

→ Set the log output verbosity for icing solvers. Default is  (minimal), set to  (Complete) to get addi-

tional information on the solver execution.

flow/ commands (FENSAP only. Use Fluent text commands for the Fluent airflow solver).

– init

→ Starts and initialize the solver.

→ This is automatically done when running calculate() for the first time, or by running calculate()

after running the solver from another mode (FENSAP airflow, particles, ice or grid displacement).

– calculate

→ Calculate FENSAP airflow for the number of iterations currently set-up in the flow/niter variable.

→ Multiple calculate commands can be executed, continuing the computation already started.

→ Example . : Use the Icing/Settings/Set Command to Set the Number of Iterations

Icing/settings/set flow/niter

→ end

Release solver memory

drop/ commands (Particles solver)

– init, calculate, end (Similar to flow/ commands)

→ The number of iterations is in drop/niter setting.

ice/ commands

– run

→ Runs the icing solver (and/or grid displacement)

The total time is in the setting ice/ice_total_time

– end

→ Release solver memory

multishot/ commands

– run

→ Runs the currently configured multishot

If icing settings are not part of your original case file, the command (load-fensapice) can be used to

enable the icing solver commands and to display the icing/ menu. A case file set-up with the Icing

application will automatically load the icing module when it is read.

Note

The full set-up and execution of the icing settings through text commands is possible since

all the icing settings are stored as rpvars and thread variables.

Interrupting a computation

On the interactive terminal of FENSAP, Ctrl+C will stop the computation at the end of the current it-

eration. When running in batch mode, the abort file (*.abort) can be used. The abort file is a simple

text file containing the “stop” keyword.

For example, for casefilename.cas

echo stop > casefilename.abort

This will interrupt the solver at the end of the current time step, this will not trigger a journal file error

and the execution will continue to the next steps.

In addition to the graphical user interface, the meshing mode of ANSYS Fluent also consists of a textual

command line reference.

The text user interface (TUI) is written in a dialect of Lisp called Scheme. Users familiar with Scheme

will be able to use the interpretive capabilities of the interface to create customized commands. The

TUI is described in the following sections:

..Text Menu System

..Text Prompt System

.. Interrupts

.. System Commands

..Text Menu Input from Character Strings

.. Using the Text Interface Help System

The text menu system provides a hierarchical interface to the program’s underlying procedural interface.

You can easily manipulate its operation with standard text-based tools: input can be saved in files, modified

with text editors, and read back in to be executed, because it is text based.

The text menu system is tightly integrated with the Scheme extension language, so it can easily be pro-

grammed to provide sophisticated control and customized functionality.

Note

The console also contains an automatic-completer feature that shows the valid inputs as

soon as you begin typing so that you can quickly enter your intended commands. This feature

can be turned on/off in Preferences.

The menu system structure is similar to the directory tree structure of LINUX operating systems. When

you first start Fluent, you are in the "root" menu and the menu prompt is simply a caret/greater-than

symbol:

>

To generate a listing of the submenus and commands in the current menu, press Enter. The available

submenus and commands will depend on whether you are running Fluent in meshing mode or solution

mode.

mode.

For instance, the submenus and commands that are available from the root menu of the solution mode

>Enter

adapt/                  mesh/                  surface/

define/                 parallel/              switch-to-meshing-mode

display/                plot/                  views/

exit                    report/

file/                   solve/

By convention, submenu names end with a / to differentiate them from menu commands. To execute

a command, type its name (or an abbreviation). Similarly, to move down into a submenu, enter its name

or an abbreviation. When you move into the submenu, the prompt will change to reflect the current

menu name.

> display

/display > set

/display/set >

To move back to the previously occupied menu, type q or quit at the prompt.

/display/set > q

/display

You can move directly to a menu by giving its full pathname.

/display > /file

/display//file >

In the above example, control was passed from /display to /file without stopping in the root

menu. Therefore, when you quit from the /file menu, control will be passed directly back to /dis-

play.

/display//file > q

/display >

If you execute a command without stopping in any of the menus along the way, control will again be

returned to the menu from which you invoked the command.

/display /file start-journal jrnl

/display >

The text menu system provides online help for menu commands. The text menu online help system is

described in Using the Text Interface Help System (p. ).

To edit the current command, you can position the cursor with the left and right arrow keys, delete

with the Backspace key, and insert text simply by typing.

For additional information, refer to the following sections:

... Command Abbreviation

... Command Line History

... Scheme Evaluation

To select a menu command, you need not type the entire name; you can type an abbreviation that

matches the command.

Text User Interface

A command name consists of "phrases" separated by hyphens.

A command is matched by matching an initial sequence of its phrases.

Matching of hyphens is optional.

A phrase is matched by matching an initial sequence of its characters.

A character is matched by typing that character.

The rules for "matching" a command are:

If an abbreviation matches more than one command, then the command with the greatest number of

matched phrases is chosen.

If more than one command has the same number of matched phrases, then the first command to appear

in the menu is chosen.

For example, each of the following will match the given command set-ambientcolor: set-

ambient-color, s-a-c, sac, and sa.

When abbreviating commands, sometimes your abbreviation will match more than one command. In such

cases, the first command is selected.

Occasionally, there is an anomaly such as lint not matching lighting-interpolation because the

li gets absorbed in lights-on? and then the nt does not match interpolation.

This can be resolved by choosing a different abbreviation, such as liin, or l-int.

You can use the up and down arrow keys on your keyboard to go through recently used commands

that are stored in history. By default, command-history will store only the last ten commands. This can

be changed (for example to ) by using the following command:

> (set! *cmd-history-length* )

Important

Command-history is not available if the ANSYS Fluent application is started with -g options

(see Command Line Startup Options in the Fluent User's Guide).

Important

The user inputs supplied as the arguments of the TUI command or alias will not be saved

in history. By way of illustration, consider the following entry in the TUI:

Text Menu System

> rc new_file.cas

Important

In history, only rc (an alias for read-case) will be saved, since new_file.cas is a user

input to the alias-function.

Commands recalled from history can be edited or corrected using the Backspace key and the left and

right arrow keys.

If you enter an open parenthesis, (, at the menu prompt, then that parenthesis and all characters up

to and including the matching closing parenthesis are passed to Scheme to be evaluated, and the

result of evaluating the expression is displayed.

> (define a )

a

> (+ a   )

Command aliases can be defined within the menu system. As with the Linux csh shell, aliases take

precedence over command execution. The following aliases are predefined in Cortex: error, pwd,

chdir, ls, ., and alias.

error

displays the Scheme object that was the “irritant” in the most recent Scheme error interrupt.

pwd

prints the working directory in which all file operations will take place.

chdir

will change the working directory.

ls

lists the files in the working directory.

. (period)

pwd

chdir

ls

. (period)

prompts you for a journal file name and then run the journal file you have specified.

alias

displays the list of symbols currently aliased.

Commands require various arguments, including numbers, filenames, yes/no responses, character strings,

and lists. A uniform interface to this input is provided by the text prompt system. A prompt consists of

a prompt string, followed by an optional units string enclosed in parentheses, followed by a default

value enclosed in square brackets. The following shows some examples of prompts:

filled-mesh? [no] Enter

shrink-factor [.] Enter

line-weight [] Enter

title [""]Enter

The default value for a prompt is accepted by pressing Enter on the keyboard or typing a , (comma).

Important

Note that a comma is not a separator. It is a separate token that indicates a default value.

The sequence “ ,” results in three values; the number  for the first prompt, the default

value for the second prompt, and the number  for the third prompt.

A short help message can be displayed at any prompt by entering a ?. (See Using the Text Interface

Help System (p. ).)

To abort a prompt sequence, simply press Ctrl+c.

... Numbers

The most common prompt type is a number. Numbers can be either integers or real numbers. Valid

numbers are, for example, , -., .9e5, and +1e-.

Integers can also be specified in binary, octal, and hexadecimal form.

The decimal integer  can be entered as , #b11111, #o37, or #x1f.

In Scheme, integers are a subset of reals, so you do not need a decimal point to indicate that a number is

real;  is just as much a real as ..

If you enter a real number at an integer prompt, any fractional part will be truncated. For example, .

will become .

... Booleans

Some prompts require a yes-or-no response. A yes/no prompt will accept either yes or y for a positive

response, and no or n for a negative response. Yes/no prompts are used for confirming potentially

dangerous actions such as overwriting an existing file, exiting without saving case, data, mesh, and so

on.

Some prompts require actual Scheme Boolean values (true or false). These are entered with the Scheme

symbols for true and false, #t and #f.

Text Prompt System

... Strings

Character strings are entered in double quotes, for example, “red”. Plot titles and plot legend titles

are examples of character strings. Character strings can include any characters, including blank spaces

and punctuation.

... Symbols

Symbols are entered without quotes. Zone names, surface names, and material names are examples

of symbols. Symbols must start with an alphabetical character (that is, a letter), and cannot include

any blank spaces or commas.

You can use wild cards to specify zone names when using the TUI. Some examples are:

* will translate as “all zones”.

– /display/boundary-grid * enables you to display all the boundary zones in the mesh.

– /boundary/delete-island-faces wrap* enables you to delete island faces on all zones

prefixed by wrap.

> will translate as “all zones visible in the graphics window”.

For example, /boundary/manage/delete >, yes enables you to delete all visible zones.

^ will translate as “all zones selected in the graphics window”.

For example, /boundary/manage/delete ^, yes enables you to delete all selected zones.

[object_name will translate as “all zones with the name object_name”.

For example, /boundary/manage/delete [box, yes enables you to delete all zones of an

object with the name box.

[object_name/label_name will translate as "all zones with label_name of object_name"

For example, /boundary/manage/delete [fluid/box*, yes enables you to delete all

zones of an object with the name fluid and comprising face zone labels box*.

If you use a wild card for an operation that requires a single zone as input, you will be prompted to

specify a single zone from the list of those that match the expression specified.

> /boundary/manage/name wall*  <Enter>

wall- wall- wall-

Zone Name [ ]

... Filenames

Filenames are actually just character strings. For convenience, filename prompts do not require the

string to be surrounded with double quotes. If, for some exceptional reason, a filename contains an

embedded space character, then the name must be surrounded with double quotes.

One consequence of this convenience is that filename prompts do not evaluate the response. For ex-

ample, the sequence

> (define fn "valve.ps")

fn

> hc fn

will end up writing a picture file with the name fn, not valve.ps. Since the filename prompt did

not evaluate the response, fn did not get a chance to evaluate “valve.ps” as it would for most

other prompts.

... Lists

... Lists

Some functions in ANSYS Fluent require a “list” of objects such as numbers, strings, Booleans, and so

on. A list is a Scheme object that is simply a sequence of objects terminated by the empty list, ’().

Lists are prompted for an element at a time, and the end of the list is signaled by entering an empty

list. This terminating list forms the tail of the prompted list, and can either be empty or can contain

values. For convenience, the empty list can be entered as () as well as the standard form ’(). Normally,

list prompts save the previous argument list as the default. To modify the list, overwrite the desired

elements and terminate the process with an empty list. For example,

element() [()]

element() [()] Enter

creates a list of three numbers: , , and . Subsequently,

element() [] Enter

adds a fourth element. Then

element() [] ()

leaves only  and  in the list. Subsequently entering

element() [] ,,’(  )

creates a five element list: , , , , and . Finally, a single empty list removes all elements

A different type of list, namely, a “list-of-scalars” contains pick menu items (and not list items) for which

a selection has to be made from listed quantities, which are available at the Enter prompt. Hence, a

list-of-scalars cannot be entered as a list.

An example of a “list-of-scalars” consists of the following:

... Evaluation

All responses to prompts (except filenames, see above) are evaluated by the Scheme interpreter before

they are used. You can therefore enter any valid Scheme expression as the response to a prompt. For

example, to enter a unit vector with one component equal to / (without using your calculator),

/foo> set-xy

x-component [.] (/  )

y-component [.] (sqrt (/  ))

or, you could first define a utility function to compute the second component of a unit vector,

> (define (unit-y x) (sqrt (- . (* x x))))

unit-y

y-component [.] (unit-y (/  ))

... Default Value Binding

The default value at any prompt is bound to the Scheme symbol “ _” (underscore) so that the default

value can form part of a Scheme expression. For example, if you want to decrease a default value so

that it is one-third of the original value, you could enter

shrink-factor [.] (/ _ )

The execution of the code can be halted by pressing the Ctrl+c, at which time the present operation

stops at the next recoverable location.

The way you execute system commands with the ! (bang) shell escape character will be slightly different

for Linux and Windows systems.

... System Commands for LINUX-based Operating Systems

... System Commands for Windows-based Operating Systems

If you are running ANSYS Fluent under a Linux-based operating system, all characters following the !

up to the next newline character will be executed in a subshell. Any further input related to these

system commands must be entered in the window in which you started the program, and any screen

output will also appear in that window. (Note that if you started ANSYS Fluent remotely, this input

and output will be in the window in which you started Cortex.)

> !rm junk. *

> !vi script.rp

!pwd and !ls will execute the Linux commands in the directory in which Cortex was started. The

screen output will appear in the window in which you started ANSYS Fluent, unless you started it re-

motely, in which case the output will appear in the window in which you started Cortex. (Note that

!cd executes in a subshell, so it will not change the working directory either for ANSYS Fluent or for

Cortex, and is therefore not useful.) Typing cd with no arguments will move you to your home directory

System Commands

ANSYS Fluent includes three system command aliases (pwd, ls, and chdir) that will be executed in

your working directory with output displayed in the ANSYS Fluent console. Note that these aliases will

invoke the corresponding Linux commands with respect to the parent directory of the case file. For

example, pwd prints the parent directory of the case file in the ANSYS Fluent console, while !pwd

prints the directory from which you started ANSYS Fluent in the Linux shell window where you started

Several examples of system commands entered in the console are shown below. The screen output

that will appear in the window in which ANSYS Fluent was started (or, if you started the program re-

motely, in the window in which Cortex was started) follows the examples.

Example input (in the ANSYS Fluent console):

> !pwd

> !ls valve*. *

> !pwd

Example output (in the window in which ANSYS Fluent— or Cortex, if you started the program re-

motely—was started):

/home/cfd/run/valve

valve1.cas  valve1.msh  valve2.cas  valve2.msh

If you are running ANSYS Fluent under a Windows operating system, all characters following the ! up

to the next newline character will be executed. The results of a command will appear in the ANSYS

Fluent console, or in a separate window if the command starts an external program, such as Notepad.

> !del junk. *

> !notepad script.rp

!cd and !dir will execute the DOS commands and the screen output will appear in the ANSYS Flu-

ent console. The !cd command with no argument will display the current working directory in the

Several examples of system commands entered in the console are shown below.

Example input (in boxes) and output (in the ANSYS Fluent console):

> !cd

p:/cfd/run/valve

> !dir valve*. */w

Volume in drive P is users

Volume Serial Number is -

Directory of p:/cfd/run/valve

valve1.cas      valve1.msh      valve2.cas      valve2.msh

File(s)              , bytes

Dir(s)          ,,, bytes free

When writing a Scheme extension function for ANSYS Fluent, it is often convenient to be able to include

menu commands in the function. This can be done with ti-menu-load-string. For example, to

open graphics window , use

(ti-menu-load-string "di ow ")

A Scheme loop that will open windows  and  and display the front view of the mesh in window

and the back view in window  is given by

(for-each

(lambda (window view)

(ti-menu-load-string (format #f "di ow ~a gr view rv ~a"

window view)))

’( )

’(front back))

This loop makes use of the format function to construct the string used by menu-load-string.

This simple loop could also be written without using menu commands at all, but you need to know

the Scheme functions that get executed by the menu commands to do it:

(for-each

(cx-open-window window)

(display-mesh)

(cx-restore-view view))

’( ) ’(front back))

String input can also provide an easy way to create aliases within ANSYS Fluent. For example, to create

an alias that will display the mesh, you could type the following:

(alias ’dg (lambda () (ti-menu-load-string "/di gr")))

Then any time you enter dg from anywhere in the menu hierarchy, the mesh will be drawn in the active

window.

Important

ti-menu-load-string evaluates the string argument in the top level menu. It ignores

any menu you may be in when you invoke ti-menu-load-string.

As a result, the command

(ti-menu-load-string "open-window  gr") ; incorrect usage

will not work even if you type it from within the display/ menu—the string itself must

cause control to enter the display/ menu, as in

(ti-menu-load-string "display open-window  mesh")

Text Menu Input from Character Strings

The text user interface provides context-sensitive online help. Within the text menu system, you can

obtain a brief description of each of the commands by entering a ? followed by the command in

question.

Example:

> ?dis

question.

Example:

> ?dis

display/: Enter the display menu.

You can also enter a lone ? to enter “help mode.” In this mode, you need only enter the command or

menu name to display the help message. To exit the help mode type q or quit as for a normal menu.

Example:

> ?

[help-mode]> di

[help-mode]> pwd

pwd: #[alias]

(LAMBDA ()

(BEGIN

(SET! pwd-cmd ((LAMBDA n

n) ’system (IF (cx-send ’(unix?))

"pwd"

"cd")))

(cx-send pwd-cmd)))

[help-mode]> q

To access the help, type a ? at the prompt when you are prompted for information.

Example:

> display/annotate Annotation text [""] ?

Annotation text [""]

Appendix A.Text Command List Changes in ANSYS Fluent  R3

For a complete listing of changes to the Text Command List for ANSYS Fluent  R3, refer to Text

Command Changes in ANSYS Fluent  R3 in the Fluent Migration Manual.

The section describes the text command listing for Fluent in Meshing mode.

boundary/ (p. ) lists the commands used for creating, managing, modifying, deleting boundary (face)

zones and surface mesh.

cad-assemblies/ (p. ) lists commands used to interact with your CAD model.

diagnostics/ (p. ) lists commands used to find and repair face zone problems related to connectivity

and quality.

display/ (p. ) lists commands used to control the rendering of your model and mesh in the graphical

window.

exit (p. ) lists the command to close the program.

file/ (p. ) lists commands used to input and output your data.

material-point/ (p. ) lists commands used to manage material points in your model.

mesh/ (p. ) lists commands used to create, manage, modify and delete cell zones and volume mesh.

objects/ (p. ) lists commands used in the object-based meshing workflow, from CAD import to volume

fill.

parallel/ (p. ) lists commands specific to parallel processing.

report/ (p. ) lists commands used to return volume and surface mesh statistics such as counts or

quality.

scoped-sizing/ (p. ) lists commands used to create and manage scoped size controls.

size-functions/ (p. ) lists commands used to create and manage size functions such as global or

periodic sizes.

switch-to-solution-mode (p. ) lists the command to transfer your mesh data to the Fluent solver.

Appendix A: Query and Utility Functions (p. ) lists API functions used to interact with your model by

passing information such as names or lists of zones or objects, statistics, and diagnostics. Boolean operations

and examples are included.

Appendix B: Boundary Functions (p. ) lists API functions used to manage boundary (face) zone mesh. Ex-

amples are included.

Appendix C: Connect Functions (p. ) lists API functions used to manage boundary (face) zone connectivity.

Examples are included.

Appendix D: Size Field Functions (p. ) lists API functions used to manage geodesic size controls and size

fields. Examples are included.

Appendix E:Wrap Functions (p. ) lists API functions used to manage your mesh in UTM cases. Examples

are included.

Chapter : boundary/

auto-slit-faces

slits all boundary faces with cells on both sides (these cells must be in the same cell zone). A displacement

can be specified to provide thickness to the boundary.

boundary-conditions/

contains options for copying or clearing boundary conditions when a case file is read.

clear

clears the boundary conditions assigned to the specified face zones.

clear-all

clears the boundary conditions assigned to all the face zones.

copy

enables you to copy the boundary conditions from the face zone selected to the face zones specified.

check-boundary-mesh

reports the number of Delaunay violations on the triangular surface mesh and the number of isolated

nodes.

check-duplicate-geom

displays the names of the duplicate surfaces and prints maximum and average distance between them.

clear-marked-faces

clears marked faces.

clear-marked-nodes

clears nodes that were marked using the mark-duplicate-nodes command.

compute-bounding-box

computes the bounding box for the zones specified.

count-free-nodes

reports the number of boundary nodes associated with edges having only one attached face.

count-marked-faces

reports the number of marked faces.

count-unused-bound-node

counts the unused boundary nodes in the domain.

count-unused-faces

lists the number of boundary faces that are not used by any cell.

count-unused-nodes

lists the number of boundary nodes that are not used by any cell.

create-bounding-box

creates the bounding box for the specified zones.You can specify the zone type, name, edge length, and

the extents of the box, as required.You can also optionally create a geometry object from the bounding

box created.

create-cylinder

creates a cylinder by specifying the axis, radius, and edge length or three arc nodes, the axial delta, the

radial gap, and the edge length.You can also specify the prefix for the zone being created, as required.

You can also optionally create a geometry object from the cylinder created.

create-plane-surface

creates a plane surface by specifying either the axis direction, axial location, and the extents of the surface

or three points defining the plane.You can also optionally create a geometry object from the plane surface

created.

create-revolved-surface

creates a revolved surface by rotating the specified edge through the angle specified. Specify the number

of segments, scale factor, and the pivot point and axis of rotation.You can also optionally create a geometry

object from the revolved surface created.

create-swept-surface

creates a surface by sweeping the specified edge in the direction specified.You need to specify the distance

to sweep through and the number of offsets, as required.You can also optionally create a geometry object

from the swept surface created.

delete-all-dup-faces

searches for faces on all boundary zones that have the same nodes and deletes the duplicates.

delete-duplicate-faces

searches for faces on a specified zone that have the same nodes and deletes the duplicates.

Duplicate faces may be present if you generated the boundary mesh using a third-party grid gener-

ator, or if you have used the slit-boundary-face command to modify the boundary mesh

and then merged the nodes.

delete-free-edge-faces

enables you to remove faces with the specified number of free edges from the specified boundary zones.

delete-island-faces

enables you to delete faces in a non-contiguous region of a face zone.

delete-unconnected-faces

enables you to delete the unconnected face-zones.

delete-unused-faces

deletes all the boundary faces that are not used by any cell.

deletes the boundary nodes that are not used by any boundary faces.

edge-limits

prints the length of the shortest and longest edges on the boundary.This information is useful for setting

initial mesh parameters and refinement controls.

boundary/

face-distribution

reports the distribution of face quality in the text window.

face-skewness

lists the worst face skewness.

feature/

enables you to create and modify features.

copy-edge-zones

copies the specified edge zone(s) to new edge zone(s).

create-edge-zones

extracts edge loops for the specified face zone(s) based on the feature method specified.You also

need to specify an appropriate value for feature angle when using the fixed-angle method.

Note

The Face Seed approach cannot be used when creating edge loops using text com-

mands.

delete-degenerated-edges

deletes degenerated edges (edges where the two end nodes are the same) for the edge zone(s) specified.

delete-edge-zones

deletes the specified edge zone(s)

edge-size-limits

reports the minimum, maximum, and average edge length for the specified edge zone(s) in the console.

group

associates the specified edge zone(s) with the specified face zone.

intersect-edge-zones

group

intersects the specified edge loops to create a new edge loop comprising the common edges.You

can enable automatic deleting of overlapped edges and specify an appropriate intersection tolerance.

list-edge-zones

lists the name, ID, type, and count for the specified edge zone(s).

merge-edge-zones

merges multiple edge loops of the same type into a single loop.

orient-edge-direction

orients the edges on the loop to point in the same direction.

project-edge-zones

projects the edges of the specified loop onto the specified face zone using the specified projection

method.

remesh-edge-zones

remeshes the specified edge loop(s), modifying the node distribution according to the specified

remeshing method, spacing values, and feature angle.You can also enable quadratic reconstruction,

if required.

reverse-edge-direction

reverses the direction of the edge loop.

separate-delete-small-edges

separates the edge zones based on the feature angle specified, and then deletes the edges having a

count smaller than the minimum count specified.

separate-edge-zones

separates the specified edge loop based on connectivity and the specified feature angle.

separate-edge-zones-by-seed

separates the edge loop based on the seed edge specified.The edge zone separation angle is used to

separate the edge zone (default ).

toggle-edge-type

toggles the edge type between boundary and interior.

ungroup

ungroups previously grouped edge zones.

fix-mconnected-edges

resolves multi-connected edges/non-manifold configurations in the boundary mesh by deleting fringes

ungroup

and overlaps based on threshold values specified.

improve/

enables you to improve boundary surfaces.

collapse-bad-faces

enables you to collapse the short edge of faces having a high aspect ratio or skewness in the specified

face zone(s).

degree-swap

enables you to improve the boundary mesh by swapping edges based on a node degree value other

than .The node degree is defined as the number of edges connected to the node.

improve

enables you to improve the boundary surface quality using skewness, size change, aspect ratio, or area

as the quality measure.

smooth

enables you to improve the boundary surface using smoothing.

swap

enables you to improve the boundary surface using edge swapping.

jiggle-boundary-nodes

randomly perturbs all boundary nodes based on an input tolerance. Some nodes will be perturbed less

than the tolerance value, while others will be perturbed by half of the tolerance value in all three coordinate

make-periodic

enables you to make the specified boundaries periodic.You can specify the type of periodicity (rotational

or translational), the angle, pivot, and axis of rotation, for rotational periodicity or the translational shift

for translational periodicity.

boundary/

For each of the zones specified, a corresponding periodic shadow boundary zone will be created.

manage/

contains options for manipulating the boundary zones.

auto-delete-nodes?

specifies whether or not unused nodes should be deleted when their face zone is deleted.

change-prefix

enables you to change the prefix for the specified face zones.

copy

copy

copies all nodes and faces of the specified face zone(s).

create

creates a new face zone.

delete

deletes the face zone.

flip

reverses the normal direction of the specified boundary zone(s).

id

specifies a new boundary zone ID. If there is a conflict, the change will be ignored.

list

prints information about all boundary zones.

merge

merges face zones.

name

gives a face zone a new name.

orient

consistently orients the faces in the specified zones.

origin

specifies a new origin for the mesh, to be used for face zone rotation and for periodic zone creation.

The default origin is (,,).

remove-suffix

removes the suffix (characters including and after the leftmost ":") in the face zone names.

rotate

rotates all nodes of the specified face zone(s).

rotate-model

rotates all nodes of the model through the specified angle, based on the specified point and axis of

rotation.

scale

scales all nodes of the specified face zone(s).

scale-model

scales all nodes of the model by multiplying the node coordinates by the specified scale factors (x, y,

z).

translate

translates all nodes of the specified face zone(s).

translate-model

translates all nodes of the model by the specified translation offsets (x, y, z).

Note

The translation offsets are interpreted as absolute numbers in meshing mode. In

solution mode, however, the translation offsets are assumed to be distances in the

length unit set. This may lead to differences in domain extents reported after trans-

lating the mesh in the respective modes.

type

changes the boundary type of the face zone.

Note

type

Note

When changing the boundary type of any zone to type interior, ensure that there

is a single cell zone across the interior boundary. Retaining multiple cell zones

across an interior boundary can cause undesirable results with further tet meshing

or smoothing operations.

interior.

The mesh check will issue a warning if multiple cell zones are maintained across an

interior boundary. The boundary type in such cases should be set to internal

instead.

user-defined-groups

enables you to manipulate user-defined groups.

activate

activates the specified user-defined groups.

create

creates the user-defined group comprising the specified zones.

delete

deletes the specified user-defined group.

list

lists the groups in the console.

update

enables you to modify an existing group.

boundary/

mark-duplicate-nodes

marks duplicate nodes.The marked nodes will appear in the grid display when nodes are displayed. For

a list of duplicate nodes, set the /report/verbosity level to  before using the mark-duplicate-

nodes command.

mark-face-intersection

marks intersecting faces. Intersection is detected if the line defined by any two consecutive nodes on a

face intersects any face in the current domain.The marked faces will appear in the grid display when faces

are displayed. For a list of intersecting faces, set the /report/verbosity level to  before using the

mark-face-intersection command.

mark-face-proximity

marks faces that are in proximity to each other.

Face A is considered to be in proximity to face B if any of the nodes on face A are within the calcu-

lated proximity distance from face B. The proximity distance is calculated based on the specified

relative distance and the sphere radius. The sphere radius is determined by the maximum distance

from the centroid of the face to its nodes. The marked faces will appear in the grid display when

faces are displayed.

For a list of faces in proximity to each other, set the /report/verbosity level to  before using

the mark-face-proximity command.

mark-faces-in-region

marks the faces that are contained in a specified local refinement region.

merge-nodes

merges duplicate nodes.

merge-small-face-zones

merges the face zones having area less than the minimum area.

modify/

contains commands used to modify the boundary mesh.

analyze-bnd-connectvty

finds and marks free edges and nodes and multiply-connected edges and nodes.This process is neces-

sary if the boundary mesh has been changed with Scheme functions.

clear-selections

clears all selections.

clear-skew-faces

clears faces that were marked using the mark-skew-face command.

collapse

collapses pairs of nodes, edge(s), or face(s). If a pair of nodes is selected, both the nodes are deleted

and a new node is created at the midpoint of the two nodes. If a triangular face is selected, the complete

face is collapsed into a single node at the centroid of the face.

create

creates a boundary face if the selection list contains  nodes and an optional zone. If the selection list

contains positions, then nodes are created.

create-mid-node

creates a node at the midpoint between two selected nodes.

delete

delete

deletes all selected faces and nodes.

delta-move

moves the selected node by specified magnitude.

deselect-last

removes the last selection from the selection list.

hole-feature-angle

specifies the feature angle for consideration of holes in the geometry.

list-selections

lists all of the selected objects.

local-remesh

remeshes marked faces or faces based on selections in the graphics window. Select the faces to be

remeshed and specify the sizing source (constant-size, geometry, or size-field), the number

of radial layers of faces to be remeshed (rings), the feature angle to be preserved while remeshing

the selected faces, and the size for constant size remeshing (if applicable).

mark-skew-face

marks faces that should be skipped when the worst skewed face is reported using the Modify

Boundary dialog box.This enables you to search for the next skewed face.

merge

merges pairs of nodes.The first node selected is retained, and the second is the duplicate that is

merged.

move

moves the selected node to the selected position if the selection list contains a node and a position.

next-skew

finds the triangular face of nearest lower skewness value than that of the worst skewed face.The face

ID, its skewness, the longest edge ID, and the node ID opposite to the longest edge are displayed in

the console.

repair

repairs zones by filling all holes associated with free faces. Specify the face zones for the repair operation.

repair-options/

contains

rezone

moves the selected faces from their current zone into the selected zone, if the selection list contains

a zone and one or more faces.

select-entity

contains

rezone

adds a cell, face, or node to the selection list by entering the name of the entity.

boundary/

select-filter

selects a filter.The possible filters are off, cell, face, edge, node, zone, position, object,

and size. If off is chosen, then when a selection is made, it is first checked to see if it is a cell, then

a face, an edge, and so on.When the node filter is used, and if a cell or face is selected, the node closest

to the selection point is picked.Thus, the nodes do not have to be displayed, to be picked.

select-position

adds a position to the selection list by entering the coordinates of the position.

select-probe

selects the probe function.The possible functions are:

box enables the selection of a group of entities within a box, to be used in conjunction with

boundary modification functions.

label prints the selection label in the graphics window

off disables the mouse probes.

polygon enables the selection of a group of entities within a polygonal region, to be used in con-

junction with boundary modification functions.

print prints the information on the selection in the console window.

select adds the selection to the selection list

select-visible-entities?

enables you to select only visible entities (nodes, edges, faces, zones, objects) when the box select or

polygon select options are used. Ensure that the model is zoomed to an appropriate level for correct

Tip

To quickly revert to the behavior of R16. or earlier, enable transparency.

Note

If the mesh is not connected, all entities (nodes, edges, faces, zones, objects) will be se-

Tip

Note

lected irrespective of whether they are visible or not.

This visual selection behavior works only on local displays and may generate warning

messages when attempting selection on a remote system.

select-zone

adds a zone to the selection list by entering the zone name or ID.

show-filter

shows the current filter.

show-probe

shows the current probe function.

skew

finds the face with the highest (worst) skewness, selects it in the graphics window, and reports its

skewness and zone ID in the console window.

skew-report-zone

enables you to select the zone for which you want to report the skewness.You can either specify zone

name or zone ID.

smooth

uses Laplace smoothing to modify the position of the nodes in the selection list. It moves the selected

node to a position computed from an average of its node neighbors.The new position is an average

of the neighboring node coordinates and is not reprojected to the discrete surface.

split-face

splits two selected faces into four faces.

swap

swaps boundary edges (of triangular faces) if the selection list contains edges.

undo

undoes the previous operation.When an operation is performed, the reverse operation is stored on

the undo stack. For example, a create operation places a delete on the stack, and a delete adds a create

The undo operation requires that the name of the object exist when the action is undone. If

the name does not exist, then the undo will fail. You can undo the last few operations, but if

many operations are being performed it is recommended that you also save the mesh periodically.

orient-faces-by-point

orients the normals based on the specified material point.

print-info

prints information about the grid in the text window.

project-face-zone

projects nodes on a selected face zone onto a target face zone. Projection can be performed based on

normal direction, closest point, or specified direction.

recover-periodic-surfaces

restores the periodic relationship between face zones. You will be prompted for the type (rotational

or translational), method (semi-automatic, automatic, or manual, depending on the periodicity type)

and for face zones. Periodicity information (angle, pivot point, axis of rotation, or translational shift)

are read in with the mesh file.

The semi-automatic option prompts you for the source boundary zones and the periodicity inform-

ation.

The automatic option prompts you for the source boundary zones.

The manual option (available only for rotational periodicity) prompts you for the source and target

boundary zones, as well as the periodicity information.

refine/

discusses the commands used to refine the boundary mesh.

boundary/

auto-refine

automatically refines a face zone based on proximity.The original face zone is treated as a background

mesh. Faces are refined by multiple face splitting passes, so that no face is in close proximity to any

face in the current domain.

clear

clears all refinement marks from all boundary faces.

count

counts the number of faces marked on each boundary zone.

limits

prints a report of the minimum and maximum size of each specified zone.This report will also tell you

count

limits

how many faces on each zone have been marked for refinement.

local-regions

enters the local refinement menu.

define

defines the refinement region according to the specified parameters.

delete

deletes the specified region.

init

creates a region encompassing the entire geometry.

list-all-regions

lists all the refinement regions in the console.

mark

marks the faces for refinement.

refine

refines the marked faces.

remesh/

has a set of commands for remeshing the face zones.

clears the highlighting of the triangles that are marked.

coarsen-and-refine

remeshes (coarsens/refines) the boundary face zones based on the computed size field. Specify the

boundary face zones to be remeshed, the boundary edge zones, feature angle, and corner angle. Ad-

ditionally, specify whether the current boundary face zones should be replaced by the remeshed face

zones after the operation is complete.

controls/

enters the edge loop tools text menu.

delete-overlapped?

toggles the deletion of region of overlap of the two surfaces.

direction

specifies the direction of the edge loop projection.

intersect/

enters the intersect control menu.

absolute-tolerance?

enables you to switch between the use of absolute and relative tolerance. By default, the relative

tolerance value is used.

delete-overlap?

enables/disables the deletion of overlapped edges. It toggles the automatic deletion of region

of overlap of the two surfaces.This option is used by while remeshing overlapping zones and

retriangulating prisms. By default, this option is enabled.

feature-angle

specifies the minimum feature angle that should be considered while retriangulating the

boundary zones. All the edges in the zone having feature angle greater than the specified

feature angle are retained.This option is useful for preserving the shape of the intersecting

boundary zones.The default value of feature angle is , however, a value in the range of

– degrees is recommended. A large value may distort the shape of the intersecting

ignore-parallel-faces?

Default is yes. If there are close-to-parallel faces, set to no to separate the zones and avoid

creating an intersection loop.

join-match-angle

specifies the allowed maximum angle between the normals of the two overlapping surfaces

to be joined.This parameter is used to control the size of the join region.

join-project-angle

specifies the allowed maximum angle between the face normal and the project direction for

the overlapping surfaces to be joined.This parameter is used to control the size of the join re-

gion.

refine-region?

enables you to refine the regions that are modified during the intersect operations. It toggles

the refinement of the intersecting regions after performing any of the intersection operation.

This operation improves the quality of the resulting mesh, however, this option is disabled

remesh-post-intersection?

used to enable or disable automatic post-remesh operation after any connect operation (join,

intersect, or stitch).

retri-improve?

enables you to improve the mesh. After performing any intersection operation, the slivers are

removed along the curve of intersection, Laplace smoothing is performed, and followed by

the edge swapping. Laplace smoothing is also performed for insert-edge-zone, remesh-

overlapped-zones, and prism-retriangulation options. Smoothing is performed

again.The smooth-swap operations can be controlled by changing the various defaults such

as swapping iterations, smoothing iterations, etc.

boundary/

separate?

enables the automatic separation of intersected zones.

stitch-preserve?

indicates that shape of the first zone specified is to be preserved.This option is enabled by

default.

tolerance

specifies the tolerance value for the intersect operations.

within-tolerance?

performs the intersection operation only within the specified tolerance value. It is useful only

for the Intersect option.

project-method

specifies the method for projecting edge loops.

proximity-local-search?

includes the selected face for proximity calculation.

quadratic-recon?

enables/disables quadratic reconstruction of edge loops.

remesh-method

specifies the method to be used for the node distribution on the edge loop.

spacing

sets the node spacing for the edge loop.

tolerance

sets the tolerance for determining if two edges intersect.

create-all-intrst-loops

creates edge loop of intersection for all boundary zones in current domain.

create-edge-loops

creates edge loops for a specified face zone, based on feature angle.

create-intersect-loop

creates an interior edge loop at the intersection between two adjacent face zones. Edges created in

this way will not be remeshed by default.

create-join-loop

creates edge loop on boundary of the region of overlap of two surfaces.

create-stitch-loop

creates edge loops for connecting two surfaces along their free edges.

delete-overlapped-edges

deletes edges that overlap selected edge loops.

faceted-stitch-zones

performs the faceted stitching of zones.

insert-edge-zone

inserts an edge zone into a triangulated boundary face zone.

intersect-all-face-zones

remeshes all the intersecting face zones.

After the intersect operation, remesh is called automatically. To disable the post-remesh operation,

use the text command:

intersect-face-zones

remeshes two intersecting face zones so that they become conformal.

join-all-face-zones

connects all overlapping face zones using the join operation.

After the join operation, remesh is called automatically. To disable the post-remesh operation,

join-face-zones

connects two overlapping faces.

mark-intersecting-faces

highlights the triangles in the neighborhood of the line of intersection.

mark-join-faces

highlights the triangles in the neighborhood of the join edge loop.

mark-stitch-faces

highlights the triangles in the neighborhood of the stitch edge loop.

remesh-face-zone

remeshes a specified face zone by automatically extracting edge loops. If edge loops are present in

the current domain (for example, if they were created using the create-edge-loops command),

they are used to remesh the specified face zone.

remesh-constant-size

remeshes the specified face zones to a constant triangle size while maintaining conformity with adjacent

zones. Specify the boundary face zones to be remeshed, the boundary edge zones, feature angle,

corner angle, and the constant size. Additionally, specify whether the current boundary face zones

should be replaced by the remeshed face zones after the operation is complete.

boundary/

remesh-face-zones-conformally

remeshes face zones using the current size function and keeping a conformal interface between them.

If no size function is defined, an error message will be generated.

This command will prompt for:

Boundary Face Zones

Boundary Edge Zones

feature angle – used to determine the minimum angle between features that will be

preserved during remeshing

corner angle – used to specify the minimum angle between feature edges that will be

preserved

Replace Face Zone? – (default is Yes) the remeshed face zone(s) will take the name and

id of the original zones, and the original face zone(s) will have “orig” appended to their name.

If No, the remeshed face zone(s) will have “retri” added postfix.

Note

Note

Periodic face zones cannot be remeshed using this command.

remesh-overlapping-zones

remeshes overlapping face zones.The non-overlapping region is remeshed using the edge loops created

from the overlapping face zones.

size-functions

enters the size functions menu where you can define size functions for controlling mesh size distribution.

compute

computes the size field based on the defined parameters.

contours/

contains options for displaying contours of size functions.

draw

displays contours in the graphics window. Compute the size field using /size-func-

tions/compute or read in a size field file prior to displaying the contours of size.

set/refine-facets?

enables you to specify smaller facets if the original are too large. Default is no.

create

defines the size function based on the specified parameters.

create-defaults

creates default size functions based on face and edge curvature and proximity.

delete

deletes the specified size function or the current size field.

deletes all the defined size functions.

disable-periodicity-filter

removes periodicity from the size field.

list

lists all the defined size functions and the parameter values defined.

reset-global-controls

resets the global controls to their default values.

set-global-controls

sets the values for the global minimum and maximum size, and the growth rate.

set-periodicity-filter

applies periodicity to the size field by selecting one source face zone.

Note

Ensure that periodicity is previously defined.

Only rotational periodicity is supported, translational periodicity is not supported

Note

currently.

set-prox-gap-tolerance

sets the tolerance relative to minimum size to take gaps into account. Gaps whose thickness is less

than the global minimum size multiplied by this factor will not be regarded as a proximity gap.

set-scaling-filter

specifies the scale factor, and minimum and maximum size values to filter the size output from

the size field.

triangulate-quad-faces?

identifies the zones comprising non-triangular elements and uses a triangulated copy of these

zones for computing the size functions.

use-cad-imported-curvature?

enables/disables curvature data from the nodes of the CAD facets.

stitch-all-face-zones

connects (stitches) all the face zones along the free edges.

After the stitch operation, remesh is called automatically. To disable the post-remesh operation,

stitch-face-zones

connects two surfaces along their free edges.

boundary/

stitch-with-preserve-boundary

connects (stitches) a zone to another which is connected to an existing volume mesh, while preserving

the boundary of the zones connected to the volume mesh. Specify a list of boundary zones to be

preserved, a list of the boundary zones to be connected to each of these zones, and the tolerance

value.

value.

Note

This command will not work for overlapping or partially overlapping face zones.

triangulate

triangulates quad zones.

reset-element-type

resets the element type (mixed, tri, or quad) of a boundary zone. If you have separated a mixed (tri and

quad) face zone into one tri face zone and one quad face zone, for example, each of these will be identified

as a “mixed" zone. Resetting the element type for each of these new zones will identify them as, respectively,

a triangular zone and a quadrilateral zone.

resolve-face-intersection

resolves self intersection on manifold surface meshes.

scale-nodes

applies a scaling factor to all node coordinates.You can use this command to change the units of the grid.

separate/

contains options for separating face zones.

define

enables you to define the local region.

delete

deletes the specified local region.

init

lists all the local regions defined.

sep-face-zone-by-angle

separates a boundary face zone based on significant angle.

sep-face-zone-by-cnbor

separates a boundary/interior face zone based on its cell neighbors.

sep-face-zone-by-mark

separates a boundary face zone by moving marked faces to a new zone.

sep-face-zone-by-region

separates a boundary face zone based on contiguous regions.

sep-face-zone-by-seed

separates a boundary face zone by defining a seed face on the surface.

sep-face-zone-by-seed-angle

separates faces connected to the seed face, whose normal fall within the specified cone.

sep-face-zone-by-shape

separates a boundary face zone based on the shape of the faces (triangular or quadrilateral).

set-periodicity

defines the periodicity parameters. You will be prompted for the type of periodicity (rotational or

translational). For rotational periodicity, you will be prompted for the angle and axis of rotation

parameters. For translational periodicity, you will be prompted for the shift vector components.

slit-boundary-face

slits a boundary face zone by duplicating all faces and nodes, except those nodes that are located at the

edges of the boundary zone. A displacement can be specified to provide thickness to the boundary.The

slit command only works when it is possible to move from face to face using the connectivity provided by

the cells.

You should slit the boundary face after you generate the volume mesh so that cells will not be

placed inside the gap. There may be some inaccuracies when you graphically display solution data

for a mesh with a slit boundary in ANSYS Fluent.

smooth-marked-faces

smooths the marked faces.

unmark-selected-faces

unmarks the marked selected faces.

wrapper/

enters the surface wrapper menu.

Note

This menu is no longer supported, and will be removed in a future release.

delete-all-cells?

deletes the Cartesian mesh.This command is available only after initializing the Cartesian grid.

boundary/

imprint-edges?

boundary/

imprints the wrapper surface on recovered feature edges that you recover.This command is available

only after creating the wrapper surface.

initialize

creates a Cartesian mesh of the specified parameters.

local-regions/

define

enables you to define the local refinement region.

delete

deletes the specified refinement region.

init

refine

refines the specified region according to the refinement parameters specified.

post-improve

enters the wrapper surface improvement options menu.

auto-post-improve

improves the wrapper surface using a pre-defined sequence of operations.

auto-post-wrap

performs a pre-defined sequence of post-wrapping operations on the wrapper surface.

coarsen-wrapper-surf

coarsens the wrapper surface.

filterout-far-features

deletes feature edges beyond the specified distance from the wrapper surface.

imprint-geom-surf

imprints the geometry threads on wrapper (manual zone recovery).

improve

improves the wrapper surface quality based on skewness, size change, or aspect ratio.

inflate-thin-regions

pushes apart the overlapping faces in thin regions.

post-single-surface

cleans up unmerged island regions after recovering the single surface.

recover-single-surface

recovers thin surfaces as a single surface after wrapping.

recover-zone

separates the wrapper surface into zones based on the original geometry.

remove-crossover-config

removes crossover configurations.

remove-duplicated-nodes

removes the duplicate nodes on the wrapper surface.

rename-wrapper-zones

renames the wrapper zones by specifying an appropriate prefix instead of the default prefix (wrap-).

resolve-nonmanifoldness

resolves non-manifold configurations on the wrapper surface.

resolve-self-intersection

removes the self intersecting faces.

rezone

smooths the zones separated from the wrapper surface for better representation of the geometry.

smooth-folded-faces

smooths the folded faces on the wrapper surface.

smooth-wrapper-surf

smooths the wrapper surface.

swap-wrapper-surf

swaps the nodes of the wrapper surface to improve its quality.

pre-smooth?

enables/disables smoothing of nodes during wrapping.This command is available only after initializing

the Cartesian grid.

region/

enters the regions menu.This command is available only after initializing the Cartesian grid.

draw-holes

draws the holes detected.

delete-interface

deletes the existing interface.

extract-enclosing-region

extracts the interface for the region enclosing the specified point.

extract-interface

extracts the interfaces for the specified regions.

fix-holes

fixes the specified hole(s).

list-holes

lists the existing holes.

boundary/

list-interfaces

lists the existing interfaces.

list-regions

lists the regions created during the wrapper initialization.

merge-interior-regions

merges all the interior regions. After using this command, two regions will remain, the exterior

and the merged interior region.

merge-regions

merges the specified regions.

modify-region-holes

enables you to fix or open holes related to the specified region.

open-holes

opens the specified hole(s).

refine

refines the Cartesian grid based on the zone specific sizes and local size functions.This command

is available only after initializing Cartesian grid.

refine-enclosing-region

refines the region enclosing the specified point.

refine-region

refines the specified region.

refine-zone-cells

refines the cells associated with the specified boundary zone.This command is available only after

initializing the Cartesian grid.

update-regions

updates the regions to account for the changes made to the original geometry (during manual

hole fixing).

wrap-enclosing-region

generates the wrapper surface for the region enclosing the specified point.

wrap-interface

generates the wrapper surface for the specified interface.

wrap-region

generates the wrapper surface for the specified region.This command is available only after initial-

izing the Cartesian grid.

wrapper-region-at-location

reports the region at the specified location.

set/

enters the menu to set cell parameters.

auto-draw-sizes

enables you to draw zone-specific sizes.

clear-size

clears all the zone specific size parameters.

curvature-factor

enables you to modify curvature size function sensitivity of a wrapper.

curvature?

enables you to enable or disable curvature size function.

default-face-size

enables you to specify default face size for Cartesian grid.

feature-threshold

enables you to specify critical range within which the nodes of the wrapper will be projected onto

the feature edges.

ignore-feature-skewness

specifies the critical skewness to be considered for ignoring feature lines.

ignore-self-proximity?

enables/disables the self-proximity calculation during the refinement.

list-size

lists the current zone specific sizes of the domain.

local-size-function

enables you to set local size functions.

max-refine-level

specifies the maximum refinement level permitted.

maximum-size-level

specifies the refinement level of the largest cell in the Cartesian grid.

minimum-proximity-gap

specifies the minimum proximity gap within which the proximity will be ignored.

minimum-size-level

specifies the refinement level of the smallest cell in the Cartesian grid.

number-of-size-boxes

controls the number of boxes to display, when using Draw Sizes button in the Face Size tab.

proximity-factor

enables you to modify proximity size function sensitivity of a wrapper.

proximity?

enables/disables proximity size function.

read-local-sizes

reads the zone specific sizes stated in a file.

refinement-buffer-layers

specifies the number of additional cell layers that you want to refine.

boundary/

relative-island-count

specifies a critical cell count of noise zones in a zone separation.

volume-marker

offers a volume marker manipulation for holes.

write-local-sizes

writes the zone specific sizes in a file.

zone-specific-size

enables you to specify zone specific sizes.

Chapter : cad-assemblies/

add-prefix

enables you to add a prefix to the selected entities. Specify the path for the entities and the prefix to be

added.

added.

add-to-object

enables you to add the selected CAD entities to an existing object. Specify the path for the entities to be

added and select the object to be modified.

create-objects

enables you to create new geometry/mesh objects for the selected entities. Specify the path for the entities

and if required, choose to create one object per CAD entity selected and/or retain the CAD zone granularity

for object creation. By default, a single object will be created for all entities selected and the CAD zone

granularity will not be retained. Specify the object name (if applicable), object type (geom or mesh), and

cell zone type (dead, fluid, or solid).

delete-cad-assemblies

deletes all the CAD assemblies data.

draw

displays the selected CAD entities.

draw-options/

contains additional options for displaying CAD entities.

add-to-graphics

adds the selected entities to the display in the graphics window.

draw-unlabelled-zones

displays the unlabeled zones for the selected entities in the graphics window.

remove-from-graphics

removes the selected entities from the display in the graphics window.

extract-edge-zones

enables you to extract the feature edge zone for the selected entities. Specify the path for the CAD entities

and the feature angle.

labels/

contains options for displaying and managing labels.

adds the selected labels to the display in the graphics window.

delete

deletes the selected labels.

draw

displays the selected labels.

removes the selected labels from the display in the graphics window.

rename

delete

draw

rename

enables you to rename the selected labels. Specify the path for the labels and the new name. For

multiple selections, the specified name will be used, with a suitable index as suffix. For example, spe-

cifying a new label name wall will result in entities wall., wall., etc.

manage-state/

contains options for setting the CAD entity state.

suppress

suppresses the selected CAD entities.

unlock

unlocks the selected CAD entities.

unsuppress

unsuppresses the selected CAD entities.

rename

enables you to rename the selected entities. Specify the path for the entities and the new name. For multiple

entities, the specified name will be used, with a suitable index as suffix. For example, specifying a new

name wall will result in entities wall., wall., etc.

replace-object

enables you to replace an object with the selected CAD entities. Specify the path for the entities to be

update-cad-assemblies

reimports the selected CAD entities using new parameters specified in the update-options/ menu.

update-options/

contains options for updating the CAD entities on reimport.

import-edge-zones?

enables you to import edge zones from the CAD entities on reimport. Specify an appropriate value for

one-object-per

enables you to change the CAD object granularity on reimport.

one-zone-per

enables you to change the CAD zone granularity on reimport.

tessellation

enables you to control the tessellation (faceting) during reimport.You can select either cad-faceting

or cfd-surface-mesh.

CAD faceting enables you to control the tessellation based on the CAD faceting tolerance and

maximum facet size specified.

cad-assemblies/

CFD Surface Mesh enables you to use a size field file during reimport. If you enter yes, specify

the size field file to be read. If you do not want to use a size field file, you can obtain conformal

faceting based on the underlying curve and surface curvature (using the minimum and maximum

facet sizes, and the facet curvature normal angle specified) and edge proximity (using the cells

per gap specified). You can also save the size field in a file (size field is computed based on the

specified parameters; that is, Min Size, Max Size, Curvature Normal Angle, Cells Per Gap).

Chapter : diagnostics/

face-connectivity/

contains options for fixing problems with face connectivity on the specified object face zones or boundary

add-label-to-small-neighbors

separates island object face zones from all connected neighbors and merges them to the connected

neighboring face zone label based on minimum face count specified.

fix-deviations

fixes deviations in the wrapped surface mesh by imprinting edges on the wrapped face zones. Specify

the number of imprint iterations and aggressive imprint iterations to be performed.

fix-duplicate-faces

removes duplicate faces.

fix-free-faces

removes free faces by the method selected.The methods available are:

removes free faces having the specified number of free edges.

delete-fringes

removes free face fringes based on the face count specified.

delete-skewed-faces

removes free faces based on the minimum skewness specified.

removes free faces by merging nodes within the tolerance specified.

stitch

removes free faces based on the tolerance and number of steps specified.

fix-invalid-normals

fixes invalid normals by smoothing.

Note

Zone-specific or scoped prism settings should be applied prior to using this command.

fix-islands

deletes groups of island faces based on the absolute face count specified.

fix-multi-faces

fixes multiply connected faces by a combination of deleting face fringes, overlapping faces, and dis-

connected faces. Specify the maximum number of fringe faces, overlapping faces, and multiply con-

nected edges, respectively.

fix-point-contacts

fixes non-manifold configurations by removing point contacts.

fix-self-intersections

fixes self intersecting or folded faces. For fixing folded faces by smoothing, specify whether features

should be imprinted.

fix-slivers

fixes faces based on skewness and height criteria. Height is the perpendicular distance between the

longest edge of the triangle and the opposite node.

fix-spikes

fixes spiked faces based on the spike angle specified.

fix-steps

fixes step configurations by smoothing or collapsing faces based on the angle and step width specified.

remove-label-from-small-neighbors

removes disconnected island object face zone labels by merging the specified island object face zones

to the connected neighboring face zone label based on minimum face count specified.

quality/

quality/

contains options for fixing problems related to surface mesh quality on the specified object face zones or

boundary face zones.

collapse

collapses bad quality faces based on area or skewness. For collapsing based on face area, specify the

maximum face area and relative maximum area. For collapsing based on face skewness, specify the

minimum skewness and feature angle. Additionally, specify the number of iterations and whether the

boundary should be preserved.

delaunay-swap

improves the surface mesh by swapping based on the minimum skewness value and feature angle

specified. Additionally, specify the number of iterations and whether the boundary should be preserved.

general-improve

improves the surface mesh based on aspect ratio, size change, or skewness. Specify the minimum

quality value, feature angle, number of iterations, and whether the boundary should be preserved.

smooth

improves the surface mesh by smoothing. Specify the number of smoothing iterations and whether

the boundary should be preserved.

diagnostics/

Chapter : display/

all-grid

displays the grid according to the currently set parameters.

annotate

adds annotation text to a graphics window. It will prompt you for a string to use as the annotation text,

and then a dialog box will prompt you to select a screen location using the mouse-probe button on your

mouse.

boundary-cells

displays boundary cells attached to the specified face zones.

boundary-grid

displays only boundary zones according to the currently set parameters.

center-view-on

mouse.

sets the camera target to be the center (centroid) of an entity.

clear

clears the active graphics window.This option is useful when you redo an overlay.

clear-annotation

removes all annotations and attachment lines from the active graphics window.

draw-cells-using-faces

draws cells that are neighbors for the selected faces.

draw-cells-using-nodes

draws cells that are connected to the selected nodes.

draw-face-zones-using-entities

draws cells that are connected to the selected entities.

draw-zones

draws the boundary/cell zones using the zone ID specified as input.

objects/

contains commands for displaying objects.

display-neighborhood

displays the objects that are in the neighborhood of the selected object.The neighboring objects have

to be in contact, or intersecting the selected object.

display-similar-area

displays the objects with similar area to the selected object area.

explode

explodes the objects in the geometry. (This command is valid only when the geometry is an assembled

mode.)

hide-objects

hides the selected objects in the display.

implode

implodes or assembles the objects in the geometry. (This command is available only when the geometry

is an exploded mode.)

isolate-objects

displays only the selected objects.

make-transparent

makes the geometry transparent so that internal objects are visible.This command works as a toggle

undoing the transparency of the previously selected objects.

select-all-visible

selects all the visible objects in the graphics window.

show-all

unhides all the objects in the geometry and displays them.

show-all

toggle-color-mode

toggles the colors of the geometry. In one mode geometry is colored object-wise while in the other

mode it is colored zone-wise.

toggle-color-palette

toggles the color palette of the geometry.

redisplay

redraws the grid in the graphics window.

save-picture

saves a picture file of the active graphics window.

set-grid/

contains options controlling the display of the grid.

all-cells?

enables/disables the display of all cells.

all-faces?

enables/disables the display of all faces.

all-nodes?

enables/disables the display of all nodes.

sets the lower and upper bounds of quality for cells to be displayed. Only cells with a quality measure

value (for example, skewness) within the specified range will be displayed.

default

resets the grid display parameters to their default values.

display/

sets the lower and upper bounds of quality for faces to be displayed. Only faces with a quality measure

free?

enables/disables the drawing of faces/nodes that have no neighboring face on at least one edge.

label-alignment

sets the alignment of labels that appear in the graphics window. By default, the label is centered on

the node, cell, and so on, to which the label refers.You can specify *,ˆ, v, <, > for center, top,

bottom, left, or right.You can also combine symbols—for example, "*v" for bottom center.

label-font

sets the label font. By default, all labels appear in “sans serif" font. Some other choices are roman,

typewriter, and stroked.

label-scale

scales the size of the label.

labels?

labels?

enables/disables the display of labels.

left-handed?

enables/disables the display of left-handed faces.

list

lists all the grid display settings.

marked?

enables/disables the display of marked nodes.

multi?

enables/disables the display of those faces/nodes that have more than one neighboring face on an

edge.

neighborhood

sets the x, y, and z range to be within a specified neighborhood of a specified grid object.

node-size

sets the node symbol scaling factor.

node-symbol

specifies the node symbol.

normal-scale

sets the scale factor for face normals.

normals?

enables/disables the display of face normals.

refine?

enables/disables the display of those faces that have been marked for refinement.

tagged?

enables/disables the display of tagged nodes.

unmeshed?

enables/disables the display of nodes and faces that have not been meshed.

unused?

enables/disables the display of unused nodes.

x-range

limits the display of grid objects to the specified x-range.

y-range

limits the display of grid objects to the specified y-range.

z-range

limits the display of grid objects to the specified z-range.

set-list-tree-separator

sets the separator character to be used to determine the common prefix for items listed in the selection

lists, when the tree view is used.

set/

Enables you to enter the set menu to set the display parameters.

colors/

enables you to enter the colors options menu.

axis-faces

sets the color of axisymmetric faces.

background

sets the background (window) color.

color-by-type?

colors/

enables you to specify that the entities should be colored by their type or ID.

color-by-partition?

enables you to view the partitions by color.This command applies to parallel processing.

far-field-faces

sets the color of far field faces.

foreground

sets the foreground (text and window frame) color.

free-surface-faces

sets the color of free surface faces.

graphics-color-theme

Sets the color theme for the graphics window.The color options (black, white, gray-gradient,

or workbench) are for the background display, but changing the theme also changes the default

colors for items that display in the graphics windows, like faces and edges.

highlight-color

sets the highlight color.

display/

inlet-faces

sets the color of the inlet faces.

interface-faces

sets the color of grid interface faces.

interior-faces

sets the color of the interior faces.

internal-faces

sets the color of the internal interface faces.

list

lists the colors available for the selected zone type.

outlet-faces

sets the color of the outlet faces.

overset-faces

sets the color of the overset faces.

periodic-faces

sets the color of periodic faces.

rans-les-interface-faces

sets the color of RANS/LES interface faces.

reset-colors

resets the individual grid surface colors to the defaults.

reset-user-colors

resets individual grid surface colors to the defaults.

show-user-colors

lists the current defined user colors.

skip-label

sets the number of labels to be skipped in the colormap scale.

surface

sets the color of surfaces.

symmetry-faces

sets the color of symmetric faces.

traction-faces

surface

sets the color for traction faces.

user-color

enables you to change the color for the specified zone.

wall-faces

sets color for wall faces.

edges?

enables/disables the display of face/cell edges.

filled-grid?

enables/disables the filled grid option.When a grid is not filled, only its outline is drawn.

lights/

enters the lights menu.

headlight-on?

turns the light that moves with the camera on/off.

lighting-interpolation

sets the lighting interpolation method to be used.You can choose flat, gouraud, or phong.

The first one is the most basic method, and the others are more sophisticated and provide

smoother gradations of color.

lights-on?

enables/disables the display of all lights.

set-ambient-color

sets the ambient color for the scene.The ambient color is the background light color in scene.

set-light

adds or modifies a directional, colored light.

line-weight

sets the line width factor for the window.

mouse-buttons

prompts you to select a function for each of the mouse buttons.

native-display-defaults

resets graphics window parameters to optimal settings for a local display.

Used after setting parameters for a remote display with remote-display-defaults.

overlays?

turns overlays on and off.

picture/

saves a hardcopy file of the active graphics window.

color-mode/

contains the available color modes.

color

selects full color and plots the hardcopy in color.

gray-scale

selects gray scale (i.e., various shades of gray) and converts color to gray-scale for hardcopy.

list

displays the current hardcopy color mode.

display/

mono-chrome

list

display/

selects color to monochrome (black and white) for hardcopy.

dpi

specifies the resolution in dots per inch for EPS and PostScript files.

driver/

contains the available hardcopy formats.

dump-window

sets the command to dump a graphics window to a file.

eps

sets the Encapsulated PostScript format.

jpeg

sets the JPEG image format.

list

displays the current hardcopy format.

options

enables you to set hardcopy options, such as landscape orientation, pen speed, and physical

size.The options may be entered on one line if you separate them with commas.

png

sets the PNG image format.

post-format/

contains commands for setting the PostScript driver format and save files in PS files that can

be printed quickly.

enables a raster file that may be larger than the standard raster file, but will print much

more quickly.

raster

enables a run-length encoded raster file that will be about the same size as the standard

raster file, but will print slightly more quickly.This is the default file type.

vector

post-script

sets the PostScript format.

ppm

sets the PPM format.

tiff

sets the TIFF format.

vrml

sets the VRML format.

invert-background?

enables/disables the exchange of foreground/background colors for hardcopy files.

jpeg-hardcopy-quality

controls the size and quality of how JPEG files are saved based on a scale of -, with zero being

low quality small files and  being high quality larger files.

landscape?

toggles between landscape or portrait orientation.

preview

preview

applies the settings of the color-mode, invert-background, and landscape options to the currently

active graphics window to preview the appearance of printed hardcopies.

use-window-resolution?

disables/enables the use of the current graphics window resolution when saving an image of the

graphics window. If disabled, the resolution will be as specified for x-resolution and y-res-

olution.

x-resolution

sets the width of the raster format images in pixels ( implies that the hardcopy should use the

same resolution as the active graphics window).

y-resolution

sets the height of the raster format images in pixels ( implies that the hardcopy should use the

re-render

re-renders the current window after modifying the variables in the set menu.

remote-display-defaults

adjusts graphics window parameters to optimal settings for a remote display.

Restore parameters for local display using native-display-defaults.

rendering-options/

contains the commands that enable you to set options that determine how the scene is rendered.

animation-option

enables you to specify the animation option as appropriate.

all

wireframe

uses a wireframe representation of all geometry during mouse manipulation.This is the default

option.

auto-spin?

enables mouse view rotations to continue to spin the display after the button is released.

display/

color-map-alignment

sets the color bar alignment.

device-info

prints out information about your graphics driver.

double-buffering?

display/

enables or disables double buffering. Double buffering dramatically reduces screen flicker during

graphics updates. If your display hardware does not support double buffering and you turn this

option on, double buffering will be done in software. Software double buffering uses extra memory.

driver

Changes the current graphics driver.When enabling graphics display, you have various options:

for Linux, the available drivers include opengl and x11; for Windows, the available drivers include

opengl, dx11 (for DirectX ), and msw (for Microsoft Windows).You can also disable the

graphics display window by entering null. For a comprehensive list of the drivers available to

you, press the Enter key at the driver> prompt.

Note

For any session that displays graphics in a graphics window and/or saves picture

files, having the driver set to x11, msw, or null will cause the rendering / saving

speed to be significantly slower.

face-displacement

sets the face displacement (in Z-buffer units along the camera Z-axis) for the displayed geometry

when both faces and edges are displayed simultaneously.

help-text-color

sets the color of the help text on the screen.You can select black, default, or white.

hidden-lines?

turns hidden line removal on or off.This command is available only when the color scheme is set

to classic.

Note

This command (only available when Graphics Color Theme is set to Black) is

deprecated and will be removed at a future release.

hidden-lines-method/

enables you to select the hidden line removal algorithm.

mesh-display-hlr?

enables you to remove hidden lines for surfaces that are very close together.This option should

be used only if the default algorithm does not produce suitable results.

normal-hlr-algorithm

is the default hidden line removal algorithm.

Note

These commands (only available when Graphics Color Theme is set to Black)

are deprecated and will be removed at a future release.

hidden-surface-method/

enables you to choose from among the hidden surface removal methods that are supported.These

options (listed below) are display hardware dependent.

hardware-z-buffer

painters

will show less edge-aliasing effects than hardware-z-buffer.This method is often used

instead of software-z-buffer when memory is limited.

software-z-buffer

is the fastest of the accurate software methods available (especially for complex scenes), but

it is memory intensive.

z-sort-only

hidden-surfaces?

enables/disables the display of hidden surfaces.

outer-face-cull?

enables/disables the display of outer faces.

set-rendering-options

sets the rendering options.

surface-edge-visibility

controls whether or not the mesh edges are drawn.

reset-graphics

resets the graphics system.

shrink-factor

sets shrinkage of both faces and cells. A value of zero indicates no shrinkage, while a value of one

would shrink the face or cell to a point.

styles/

contains commands for setting the display style for the different types of nodes and faces that can be

styles/

indicates cells within the specified cell quality range.

display/

cell-size

indicates cells within the specified cell size range.

indicates faces within the specified face quality range.

face-size

indicates faces within the specified face size range.

free

indicates free nodes or faces.

indicates faces that do not follow the right-hand rule with respect to their cell neighbors.

mark

indicates marked objects (for expert users).

multi

indicates multiply-connected nodes or faces.

refine

indicates boundary faces to be refined.

tag

indicates tagged objects (for expert users).

unmeshed

indicates unmeshed nodes or faces.

unused

indicates unused nodes or faces.

title

sets the problem title.

windows/

enters the windows options menu, which contains commands that enable you to customize the relative

positions of sub-windows inside the active graphics window.

The menu structure for the axes, main, scale, text, video, and xy submenus is similar.

aspect-ratio

sets the aspect ratio of the active window.

axes/

enters the axes window options menu.

border?

sets whether or not to draw a border around the axes window.

bottom

sets the bottom boundary of the axes window.

clear

sets the transparency of the axes window.

left

sets the left boundary of the axes window.

right

sets the right boundary of the axes window.

top

sets the top boundary of the axes window.

visible?

controls the visibility of the axes window.

main/

enters the main view window options menu.

border?

sets whether or not to draw a border around the main viewing window.

visible?

main/

border?

bottom

sets the bottom boundary of the main viewing window.

left

sets the left boundary of the main viewing window.

right

sets the right boundary of the main viewing window.

top

sets the top boundary of the main viewing window.

visible?

controls the visibility of the main viewing window.

scale/

enters the color scale window options menu.

border?

sets whether or not to draw a border around the color scale window.

bottom

sets the bottom boundary of the color scale window.

clear?

sets the transparency of the color scale window.

font-size

sets the font size of the color scale window.

format

sets the number format of the color scale window (for example, %.2e).

display/

left

sets the left boundary of the color scale window.

margin

sets the margin of the color scale window.

right

sets the right boundary of the color scale window.

top

sets the top boundary of the color scale window.

visible?

controls the visibility of the color scale window.

text

enters the text window options menu.

application?

shows or hides the application name in the picture.

border?

sets whether or not to draw a border around the text window.

bottom

sets the bottom boundary of the text window.

clear?

enables/disables the transparency of the text window.

company?

shows or hides the company name in the picture.

date?

shows or hides the date in the picture.

left

sets the left boundary of the text window.

right

sets the right boundary of the text window.

top

sets the top boundary of the text window.

visible?

controls the visibility of the text window.

video/

right

top

visible?

video/

contains options for modifying a video.This menu is not relevant for the meshing mode.

sets the background color of the graphics window.The color is specified as a string of three

comma-separated numbers between  and , representing red, green, and blue. For example,

to change the background from black (default) to gray, you would enter ".,.,." after selecting

the background command.

color-filter

sets the video color filter. For example, to change the color filter from its default setting to PAL

video with a saturation of % and a brightness of %, you would enter

"video=pal,sat=.,gain=." after selecting the color-filter command.

sets the foreground (text) color of the graphics window.The color is specified as a string of

three comma-separated numbers between  and , representing red, green, and blue. For ex-

ample, to change the foreground from white (default) to gray, you would enter ".,.,." after

selecting the foreground command.

on?

enables or disables the video picture settings.

pixel-size

sets the window size in pixels.

xy/

enters the XY plot window options menu.

border?

sets whether or not to draw a border around the XY plot window.

bottom

sets the bottom boundary of the XY plot window.

left

sets the left boundary of the XY plot window.

right

sets the right boundary of the XY plot window.

top

sets the top boundary of the XY plot window.

visible?

controls the visibility of the XY plot window.

update-scene/

contains commands that enable you to update the scene description.

delete

deletes the geometry selected using the select-geometry command.

delete

display

displays the geometry selected using the select-geometry command.

draw-frame?

enables/disables the drawing of the bounding frame.

overlays?

enables/disables the overlays option.

display/

select-geometry

enables you to select the geometry to be updated.

set-frame

enables you to change the frame options.

transform

enables you to apply the transformation matrix to the geometry selected using the select-geometry

command.

views/

enters the view window options menu.

auto-scale

scales and centers the current scene without changing its orientation.

camera/

contains commands to set the camera options.

dolly-camera

enables you to move the camera left, right, up, down, in, and out.

field

enables you to set the field of view (width and height) of the scene.

orbit-camera

enables you to move the camera around the target. Gives the effect of circling around the target.

pan-camera

gives you the effect of sweeping the camera across the scene.The camera remains at its position

but its target changes.

position

sets the camera position.

projection

lets you switch between perspective and orthographic views.

roll-camera

lets you adjust the camera up-vector.

target

sets the point the camera will look at.

up-vector

sets the camera up-vector.

zoom-camera

adjusts the camera’s field of view.This operation is similar to dollying the camera in or out of the

scene. Dollying causes objects in front to move past you. Zooming changes the perspective effect

in the scene (and can be disconcerting).

default-view

resets the view to front and center.

delete-view

deletes a particular view from the list of stored views.

last-view

returns to the camera position before the last manipulation.

list-views

lists all predefined and saved views.

read-views

reads views from an external view file.

restore-view

sets the current view to one of the stored views.

save-view

saves the currently displayed view into the list of stored views.

write-views

writes views to an external view file.

xy-plot/

enters the XY plot menu.

cell-distribution

plots a histogram of cell quality.

plots a histogram of face quality.

file

enables you to choose a file from which to create an xy plot.

set/

enters the set window options menu.

auto-scale?

sets the range for the x- and y-axis. If auto-scaling is not activated for a particular axis, you will be

prompted for the minimum and maximum data values.

background-color

sets the color of the field within the abscissa and ordinate axes.

file-lines

sets the parameters for plot lines.

file-markers

sets the parameters for data markers.

key

sets the visibility and title of the description box that displays the markers and/or lines with their

associated data.The key can be positioned and resized using the left mouse button.

labels

sets the strings that define the x- and y- axis labels.

display/

lines

sets the pattern, weight, and color of the plot lines.

log?

enables/disables the log scaling on the x- and y-axis.

markers

sets parameters for the data markers.

numbers

sets the format and precision of the data numbers displayed on the x- and y-axis.

plot-to-file

enables you to write the xy plot values to a file.

rules

numbers

rules

sets the visibility, line weight and color of the major and minor rules in the x- and y-axis directions.

windows

contains commands that enable you to customize the relative positions of sub-windows inside the

active graphics window.

border?

draws a border around the sub-window.

bottom

sets the bottom boundary of the sub-window.

left

sets the left boundary of the sub-window.

right

sets the right boundary of the sub-window.

top

sets the top boundary of the sub-window.

visible?

sets the visibility of the sub-window.

xy-percent-y?

enables/disables whether the y-coordinate should be scaled to show a percent of total values being

plotted.

zones/

contains commands for displaying zones.

displays the zones that are in the neighborhood of the selected zones.The neighboring zones have

to be in contact, or intersecting the selected zone.

displays the zones with similar area to the selected zone area.

hide-zones

hides the selected zones in the display.

isolate-zones

displays only the selected zones.

makes the geometry transparent so that internal zones are visible.This command works as a toggle

undoing the transparency of the previously selected zones.

selects all the visible zones in the graphics window.

show-all

unhides all the zones in the geometry and displays them.

display/

Chapter : exit

display/

exit

exits the program.

Chapter : file/

The user interface commands related to the File menu (such as reading files, importing files) and other

Select File dialog boxes do not work for the dual process build. You need to use the TUI commands

instead (for example, /file/read-mesh).

Important

need to save the data if the machine must be shut down in between.

append-mesh

enables you to append the mesh files.This command is available only after a mesh file has been read in.

If zone names and IDs are duplicated, they will be modified and the changes will be reported in the

console.

Refinement region information will be retained during the file append operation. If region names are

duplicated, they will be modified and the changes will be reported in the console.

append-meshes-by-tmerge

enables you to append the mesh files using the tmerge utility.This command is available only after a mesh

file has been read in.

confirm-overwrite?

controls whether attempts to overwrite existing files require confirmation.

If you do not want ANSYS Fluent to ask you for confirmation before it overwrites existing files, you

can enter the file/confirm-overwrite? text command and answer no.

file-format

enables/disables the writing of binary files.

filter-list

lists the names of the converters that are used to change foreign mesh (while importing mesh files from

third-party packages) files.

filter-options

enables you to change the extension (such as .cas, .msh, .neu) and arguments used with a specified filter.

For example, if you saved the PATRAN files with a .NEU extension instead of .neu, you can substitute

or add .NEU to the extension list. For some filters, one of the arguments will be the dimensionality

of the grid.

When you use the filter-options command for such a filter, you will see a default dimension-

ality argument of -d a. The dimension will automatically be determined, so you need not substitute

or  for a.

import/

enables you to import mesh information generated by some CAD packages (ANSYS, I-deas, NASTRAN,

PATRAN, and HYPERMESH), as well as mesh information in the CGNS (CFD general notation system) format.

These files are imported using the associated text commands listed here:

ansys-surf-mesh

enables you to read a ANSYS surface mesh file.

ansys-vol-mesh

enables you to read a ANSYS volume mesh file.

cad

cad

enables you to import CAD files based on the options set.

To import a single file (default), specify the file path and set up options for extracting features, im-

porting curvature data from CAD, and the length unit.

To import multiple files, specify the directory path and pattern, and set up options for appending

the files, extracting features, importing curvature data from CAD and the length unit.

cad-geometry

To import a single file (default), specify the file path. Set up options for the length unit, tessellation

method, and sizing parameters based on the tessellation method.

To import multiple files, specify the directory path and pattern. Set up options for appending the

files, the length unit, tessellation method, and sizing parameters based on the tessellation method.

cad-options/

contains additional options for importing CAD files.

continue-on-error?

enables you to continue the import of the CAD file(s), despite errors or problems creating the fa-

ceting on certain surfaces, or other issues.This option is disabled by default.

file/

create-cad-assemblies?

enables creating the CAD Assemblies tree on CAD import.The CAD Assemblies tree represents

from the CAD are maintained on import in Fluent Meshing.

For commands specific to the CAD assemblies, refer to cad-assemblies/ (p. )

derive-zone-name-from-object-scope?

enables zones without Named Selections to inherit the object name on import.This option is dis-

abled by default.

double-connected-face-label

adds the specified label to the name of double-connected face zones (face zones shared by two

bodies).

enclosure-symm-processing?

enables processing of enclosure and symmetry named selections during import.This option is

disabled by default.This option is applicable only to ANSYS DesignModeler (*.agdb) files.

extract-features?

enables feature extraction from the CAD model on import.You can choose to disable this, if desired.

Specify an appropriate value for feature angle.The default value is .

import-body-names?

enables import of Body names from the CAD files.This option is enabled by default.

Note

Any renaming of Body names in ANSYS Mechanical/ANSYS Meshing prior to the

export of the mechdat/meshdat files is ignored during import. Only original Body

names will be imported.

import-curvature-data-from-CAD?

enables importing of the curvature data from the nodes of the CAD facets.You can choose to disable

import-part-names?

enables import of Part names from the CAD file(s).This option is enabled by default.

Note

Any renaming of Part names in ANSYS Mechanical/ANSYS Meshing prior to the

export of the mechdat/meshdat files is ignored during import. Only original Part

merge-nodes?

enables the merging of geometry object nodes during CAD import.This option is enabled by default.

Note

This option can be optionally enabled/disabled only when geometry objects are

imported using the CAD Faceting option for CAD import. Mesh object nodes

will always be merged when the CFD Surface Mesh is selected for CAD import.

modify-all-duplicate-names?

enables you to modify all duplicate object/zone names by adding incremental integers as suffix.

For example: The CAD file contains multiple parts (or bodies) named heatshield.

With the option disabled (default), the imported zones will be named heatshield, heatshield.,

heatshield., etc.

With the option enabled, the imported zones will be named heatshield., heatshield., heat-

shield., etc.

name-separator-character

allows you to specify the character used between name fields. Default is ':'.

named-selections

enables you to import Named Selections from the CAD file(s), including Named Selections from

ANSYS DesignModeler, publications from CATIA, and so on.You can additionally choose to ignore

import of certain Named Selections based on the pattern specified (for example, Layer* to ignore

layer Named Selections from CATIA), or by specifying multiple wild cards (for example, ^(Col-

or|Layer|Material). * to remove color, layer, and material Named Selections from CATIA).

Note

If Named Selections is enabled, then Face named selections will be imported as face

zone labels.

object-type

enables the setting of object type on import.The options available are auto, geometry, and

mesh.The default setting is auto based on the tessellation method selected: geometry objects

will be created when the cad-faceting  method is used, while mesh objects will be created

when the cfd-surface-mesh method is used.

one-face-zone-per

enables you to create one face zone per body/face/object to be imported.

enables you to create one object per body/part/file/selection to be imported. The default

program-controlled option allows the software to make the appropriate choice. This

file/

option makes a choice between per body and per part based on whether shared topology

is off or on, respectively.

Note

For ANSYS ICEM CFD files (*.tin), set the object granularity to one object per se-

lection.

read-all-cad-in-subdirectories?

when enabled, all files in the specified directory as well as in its subdirectories will be imported.

save-PMDB?

saves a PMDB (*.pmdb) file in the directory containing the CAD files imported.You can use this

file to import the same CAD file(s) again with different options set, for a quicker import than the

full import.This option is disabled by default.

Note

Some options will not be available any more once the model is imported from

a PMDB file (for example, enclosure-symm-processing? ), since they are

processed before the PMDB file is created.

separate-features-by-type?

enables separation of feature edges based on angle, connectivity, and named selections on import.

Edge zone names will have suitable suffixes depending on separation criteria, order of zones, ex-

isting zone names and other import options selected.

single-connected-edge-label

adds the specified label to the name of single-connected edge zones (edge zones referenced by

a single face).

strip-file-name-extension-from-naming?

removes the extension of the CAD files from the object/face zone names on import.This option is

strip-path-prefix-from-names?

enables you to remove the path prefix from the object/face zone names on import.The default

setting is auto which removes the path prefix from object/face zone names when the object cre-

ation granularity is set to one object per file.You can also explicitly select yes or no.

enables you to control the tessellation (faceting) during file import.You can select either cad-

faceting or cfd-surface-mesh.

CAD faceting enables you to control the tessellation based on the CAD faceting tolerance

and maximum facet size specified.

CFD Surface Mesh enables you to use a size field file, (Use size field file?). If you

enter yes, specify the size field file to be read. If you do not want to use a size field file,

you can obtain conformal faceting based on the underlying curve and surface curvature

(using the minimum and maximum facet sizes, and the facet curvature normal angle specified)

and edge proximity (using the cells per gap specified). You can also save a size field in a file

(size field is computed based on the specified parameters; that is, Min Size, Max Size,

Curvature Normal Angle, Cells Per Gap).

use-collection-names?

enables you to use the Named Selections for the object/zone names on import. Select auto, no,

or yes.The default selection is auto where the Named Selection will be used as the object/zone

name, except when the object creation granularity is set to one object per file.

use-component-names?

enables you to add the component (part or assembly) names to the object/zone names on import.

Select auto, no, or yes.The default selection is auto where the component name will be added

to the object/zone name.

use-part-names?

enables you to choose whether to add the part names from the CAD file to the object and zone

names on import.The default setting is auto which adds the part names to both object and zone

names when object creation granularity is set to body.When the object creation granularity is set

to part or file, the part names are not added to the zone names, face zone labels, or the region

names, by default.You can also explicitly select yes or no.

use-part-or-body-names-as suffix-to-named-selections?

enables you to modify zone names by using part or body names as suffixes to the Named Selections

spanning multiple parts/bodies.This option is enabled by default.

For example: The CAD file contains a Named Selection effusion with part (or body) names

id_liner and od_liner.

With the option enabled (default), the imported zones will be named effusion:id_liner and ef-

fusion:od_liner.

With the option disabled, the imported zones will be named effusion. and effusion..

cgns-surf-mesh

enables you to read a CGNS surface mesh file.

cgns-vol-mesh

enables you to read a CGNS volume mesh file.

fidap-surf-mesh

enables you to read a FIDAP surface mesh file.

fidap-vol-mesh

enables you to read a FIDAP volume mesh file.

fl-uns2-mesh

enables you to read a Fluent UNS V2 case file.

fluent-2d-mesh

enables you to read a 2D mesh into the 3D version.

gambit-surf-mesh

enables you to read a GAMBIT surface mesh file.

file/

gambit-vol-mesh

enables you to read a GAMBIT volume mesh file.

hypermesh-surf-mesh

enables you to read a HYPERMESH surface mesh file.

hypermesh-vol-mesh

enables you to read a HYPERMESH volume mesh file.

ideas-surf-mesh

enables you to read an I-deas surface mesh file.

ideas-vol-mesh

enables you to read an I-deas volume mesh file.

nastran-surf-mesh

enables you to read a NASTRAN surface mesh file.

nastran-vol-mesh

enables you to read a NASTRAN volume mesh file.

patran-surf-mesh

enables you to read a PATRAN surface mesh file.

patran-vol-mesh

enables you to read a PATRAN volume mesh file.

load-act-tool

loads the ANSYS ACT tool.

read-boundary-mesh

enables you to read a boundary mesh. If the boundary mesh is contained in two or more separate files,

you can read them in together and assemble the complete boundary mesh.

This option is also convenient if you want to reuse the boundary mesh from a file containing a large

Note

The naming of face zones can be controlled by Named Selections defined in ANSYS

Workbench. For details on exporting faceted geometry from ANSYS Workbench, refer to

the ANSYS Workbench Help.

read-case

enables you to read the mesh contained in a case file.

Note

Cell hierarchy in case files adapted in the solution mode will be lost when they are read

in the meshing mode.

Case files containing polyhedral cells can also be read in the meshing mode of Fluent. You can

display the polyhedral mesh, perform certain mesh manipulation operations, check the mesh quality,

and so on.

read-domains

enables you to read domain files.

Each mesh file written by Fluent has a domain section. A domain file is the domain section of the

mesh file and is written as a separate file. It contains a list of node, face, and cell zone IDs that make

up each domain in the mesh.

If a domain that is being read already exists in the mesh, a warning message is displayed. Fluent

verifies if the zones defining the domains exist in the mesh. If not, it will display a warning message.

read-journal

enables you to read a journal file into the program.

The read-journal command always loads the file in the main (that is, top-level) menu, regardless

of where you are in the menu hierarchy when you invoke it.

read-mesh

enables you to read a mesh file.You can also use this command to read a Fluent mesh file created with

GAMBIT, or to read the mesh available in a Fluent case file.

Note

Reading a case file as a mesh file will result in loss of boundary condition data as the

mesh file does not contain any information on boundary conditions.

and so on.

Important

Note

Note

read-meshes-by-tmerge

uses the tmerge utility to read the mesh contained in two or more separate files. It enables you to read

the mesh files together and helps assemble the complete mesh.

read-multi-bound-mesh

enables you to read multiple boundary mesh files into the meshing mode.

file/

read-multiple-mesh

enables you to read in two or more files together and have the complete mesh assembled for you, if the

mesh files are contained in two or more separate files.

For example, if you are going to create a hybrid mesh by reading in a triangular boundary mesh

and a volume mesh consisting of hexahedral cells, you can read both files at the same time using

this command.

read-options

enables you to set the following options for reading mesh files:

consistently when the mesh file is read. If necessary, the zones being read will be separated, such that

each boundary face zone has at most two cell zones as neighbors, one on either side. Also, internal face

zones are inserted between neighboring cell zones that are connected by interior faces.

errors, no automatic mesh repair is done, and that parts of the mesh may be non-conformal, contain

voids, or be erroneous in other ways.The purpose of the check-read-data option is to enable access

to corrupt files.This option is disabled by default with the assumption that correct data will be read,

and to shorten file read times.

read-size-field

enables you to read in a size field file.

Note

If you read a size-field file after scaling the model, ensure that the size-field file is appro-

priate for the scaled model (size-field vertices should match the scaled model).

set-tui-version

Allows you to improve backwards compatibility for journal files.This command hides any new TUI prompts

that are added at a future release of ANSYS Fluent and reverts to the arguments of the release that you

specify using the command (within two full releases of the current release).The command is automatically

added to a journal file as soon as you start the recording. See Creating and Reading Journal Files for details.

show-configuration

displays the current release and version information.

start-journal

starts recording all input and writes it to a file.The current Fluent version is automatically recorded in the

journal file. Note that commands entered using paths from older versions of Fluent will be upgraded to

their current path in the journal file. See Creating and Reading Journal Files in the Fluent User's Guide.

To start the journaling process use the file/start-journal command, and end it with the

file/stop-journal command (or by exiting the program). To read a journal file into the program,

use the file/read-journal command.

Note

The read-journal command always loads the file in the main (that is, top-level) menu,

regardless of where you are in the menu hierarchy when you invoke it.

The standard period (.) alias is the same as the file/read-journal definition and is defined

by:

(alias ’. (lambda () (ti-read-journal)))

start-transcript

starts recording input and output in a file.

A transcript file contains a complete record of all standard input to and output from Fluent (usually

all keyboard and user interface input and all screen output).Start the transcription process with the

file/start-transcript command, and end it with the file/stop- transcript command

(or by exiting the program).

stop-journal

stops recording input and closes the journal file.

stop-transcript

stops recording input and output, and closes the transcript file.

write-boundaries

enables you to write the specified boundaries into a mesh file.

This is useful for large cases where you may want to mesh different parts of the mesh separately

and then merge them together. This enables you to avoid frequent switching between domains for

such cases. You can write out selected boundaries to a mesh file and then create the volume mesh

for the part in a separate session. You can then read the saved mesh into the previous session and

merge the part with the rest of the mesh.

write-case

enables you to write a case file that can be read by Fluent.

Note

Note

write-domains

enables you to write all the mesh domains (except global) into a file that can be read.

file/

write-mesh

enables you to write a mesh file.

Note

write-options

enables you to set the enforce mesh topology option for writing mesh/case files.

This option is disabled by default; enabling this option will orient the face zones consistently when

the mesh file is written. If necessary, the zones will be separated, such that each boundary face

zone has at most two cell zones as neighbors, one on either side. Also, internal face zones will be

inserted between neighboring cell zones that are connected by interior faces.

write-size-field

enables you to write a size field file.

Chapter : material-point/

create-material-point

enables the definition of a material point. Specify the fluid zone name and the location to define the ma-

terial point.

delete-all-material-points

enables the deletion of all defined material points.

delete-material-point

deletes the specified material point.

list-material-points

lists all the defined material points.

Chapter : mesh/

auto-mesh

enables you to generate the volume mesh automatically. Specify a mesh object name for object-based

auto mesh; if no name is given, face zone based auto mesh is performed. Specify the mesh elements to

be used when prompted. Specify whether to merge the cells into a single zone or keep the cell zones

separate. For face zone based meshing, specify whether automatically identify the domain to be meshed

based on the topology information.

Note

You can specify the meshing parameters for the mesh elements (prisms, pyramids or non-

conformals, tet, hex or poly) using either the respective dialog boxes or the associated text

commands prior to using the auto-mesh command.

auto-mesh-controls/

enters the auto-mesh-controls submenu

backup-object

enables creation of a backup of the surface mesh before volume meshing starts.This option is enabled

enables you to specify a prefix for cell zones created during the auto mesh procedure.

Note

The auto-prefix-cell-zones command is not relevant for object-based meshing,

where the cell zone names are generated based on the material points and the objects

used to generate the mesh object.

cavity/

enters the cavity menu.

add-zones

enables you to create a cavity for adding new zones to the existing volume mesh.

create-hexcore-cavity-by-region

creates the cavity in the hexcore mesh based on the zones and bounding box extents specified.

create-hexcore-cavity-by-scale

creates the cavity in the hexcore mesh based on the zones and scale specified.

merge-cavity

enables you to merge the specified cavity domain with the parent domain.

During the merging operation, the cavity cell zones merges with the zones in the parent domain.

The wall boundaries extracted from the interior zones will be converted to interior type and

merged with the corresponding zones in the parent domain.

region

enables you to create a cavity to modify the existing volume mesh in the specified region.

region

remove-zones

enables you to create a cavity for removing zones from the existing volume mesh.

replace-zones

enables you to create a cavity for removing a set of zones from an existing volume mesh and replacing

them with new set of zones.

cell-zone-conditions/

contains options for copying or clearing cell zone conditions when a case file is read.

clear

clears the cell zone conditions assigned to the specified zones.

clear-all

clears the cell conditions assigned to all the zones.

copy

enables you to copy the cell zone conditions from the zone selected to the zones specified.

checks the mesh for topological errors.

check-quality

enables you to ensure that the mesh quality is appropriate before transferring the mesh to the solution

mode.

check-quality-level

enables you to report additional quality metrics when set to .

In addition to the orthogonal quality and Fluent aspect ratio, additional metrics such as cell squish

and skewness will be reported when the check-quality-level is set to .

clear-mesh

enables you to generate a new mesh by deleting the internal mesh and leaving only the boundary faces

and nodes.

create-heat-exchanger

creates the heat exchanger mesh.You need to specify the method for selecting the Location coordinates

(by Position or Nodes), the location coordinates, the parameters for setting up mesh density (by Interval

or Size), and the number of intervals (sizes) between points (nodes) –, –, –. Also specify the ob-

ject/zone name prefix and enable creating the mesh object, if required.

mesh/

cutcell/

enters the cutcell menu.

Note

mesh/

cutcell/

Note

create

creates the CutCell mesh by performing the initialize, refine, snap, and improve operations sequentially.

create-prism

creates the prism layers on the recovered boundary based on the zone-specific prism parameters set.

Specify the cell zones into which the prism layers are to be grown and the gap factor as appropriate.

modify/

enters the cutcell modify menu.

auto-node-move

enables you to use the Auto Node Move utility to improve the CutCell mesh quality.

cavity-remeshing

enables you to use the Cavity Remeshing utility to improve the CutCell mesh quality near the

boundary.

Note

Face zones of type internal are recovered as type wall in the cutcell mesher.

These should be reset to type internal before using the cavity remesher.

post-morph-improve

improves the quality of the CutCell mesh post-prism generation.

rezone-multi-connected-faces

enables you to resolve multi-connected configurations on the CutCell boundary. Specify an appro-

priate value for the critical count for contiguous manifold faces.

An example is shown in Figure . : Rezoning Multiply Connected Faces (p. ) where the

multiply connected faces around the surface are removed.

split-boundary

creates a copy of the specified CutCell boundary zones and makes the boundary mesh conformal

at the hanging-nodes on the copied zones.The new zones will be named based on the original

zone names and prefixed by split-.

objects/

enters the objects menu.

change-object-type

enables you to change the object type (geom or mesh).

objects/

checks the mesh on the specified objects for connectivity and orientation of faces.The domain

extents, volume statistics, and face area statistics will be reported along with the results of other

checks on the mesh.

create

creates the object based on the priority, cell zone type, face zones, edge zones, and object type

specified.You can specify the object name or retain the default blank entry to have the object

name generated automatically.

create-and-activate-domain

creates and activates the domain comprising the face zones from the objects specified.

create-groups

creates a face group and an edge group comprising the face zones and edge zones included in

the specified objects, respectively.

create-intersection-loops

enables you to create intersection loops for objects.

The collectively option creates an interior edge loop at the intersection between two ad-

jacent face zones included in the same object and between multiple objects.

The individually option creates an interior edge loop at the intersection between two ad-

jacent face zones included in the same object.

create-multiple

creates multiple objects by creating an object per face zone specified.The objects will be named

automatically based on the prefix and priority specified.

create-new-mesh-object/

contains options for creating a new mesh object by wrapping or remeshing existing objects.

remesh

creates a new mesh object by remeshing geometry objects individually or collectively.

wrap

creates a new mesh object by wrapping the specified objects individually or collectively.

delete

deletes the specified objects.

wrap

delete

deletes all the defined objects.

mesh/

deletes all the defined geom objects.

delete-unreferenced-faces-and-edges

deletes all the faces and edges that are not included in any defined objects.

extracts the edge zones from the face zones included in the specified objects, based on the edge-

feature-angle value specified (/mesh/cutcell/objects/set/set-edge-feature-angle).

improve-feature-capture

enables you to imprint the edges comprising the object on to the object face zones to improve

feature capture for mesh objects.You can specify the number of imprinting iterations and addi-

tional aggressive imprinting iterations to be performed.

improve-object-quality

This command is not relevant for CutCell meshing.

join-intersect/

The commands in this sub-menu are not relevant for CutCell meshing.

list

lists the defined objects, indicating the respective cell zone type, priority, face zones and edge

zones comprising the object, object type, and object reference point in the console.

merge

merges the specified objects into a single object.

merge-edges

merges all the edge zones in an object into a single edge zone.

Note

If the object is composed of edge zones of different types (boundary and interior),

the edge zones of the same type (boundary or interior) will be merged into a

single edge zone.

merges the free nodes at the object level based on the specified tolerance or using a tolerance

that is a specified percentage of shortest connected edge length.

merge-voids

enables you to merge voids in the mesh object after the sewing operation.This command is not

relevant for CutCell meshing.

merges all the face zones of type wall in an object into a single face zone.

remove-gaps/

contains options for removing gaps between mesh objects.The commands in this sub-menu are

not relevant for CutCell meshing.

rotate

rotates the objects based on the angle of rotation, pivot point, and axis of rotation specified.

scale

scales the objects based on the scale factors specified.

separate-faces-by-angle

separates the face zones comprising the object based on the angle specified.

separate-faces-by-seed

separates the face zones comprising the object based on the seed face specified.

set/

contains the following options:

set-edge-feature-angle

sets the edge feature angle to be used for extracting edge zones from the face zones included

in the objects.

show-edge-zones?

displays the edge zones comprising the objects drawn in the graphics window.

show-face-zones?

displays the face zones comprising the objects drawn in the graphics window.

sew/

contains options for sewing mesh objects.The commands in this sub-menu are not relevant for

translate

translates the objects based on the translation offsets specified.

update

enables you to update the objects defined when the face and/or edge zones comprising the object

have been deleted.

wrap/

contains options for the object wrapping operation.The commands in this sub-menu are not rel-

evant for CutCell meshing.

set/

enters the CutCell settings menu.

auto-delete-dead-zones?

controls the automatic deleting of the dead zones in the CutCell mesh.

auto-delete-solid-zones?

set/

controls the automatic deleting of the solid zones in the CutCell mesh.

enables you to define a material point.

enables you to delete all defined material points.

mesh/

max-initial-cells

specifies the maximum number of cells in the initial Cartesian grid.

set-cutcell-quality-method

enables you to set the quality measure for the improve operation.The default measure used is the

orthoskew metric.

set-post-morph-parameters

enables you to set parameters for improving the CutCell mesh post-prism generation using the

command /mesh/cutcell/modify/post-morph-improve.

set-post-snap-parameters

enables you to set parameters for improving the CutCell mesh quality.

set-thin-cut-face-zones

enables you to specify the face zones constituting the thin regions to be recovered during the

CutCell meshing process.

set-thin-cut-edge-zones

enables you to specify the edge zones defining the features in thin regions to be recovered during

the CutCell meshing process.

size-functions/

enters the size functions menu.

compute

contours/

enters the contours sub-menu.

draw

create

create

delete

list

lists all the defined size functions and the corresponding parameter values defined.

list-periodicity-filter

lists the details of the source zone and rotational periodic parameters specified for the size field.

resets the values for the global controls to the defaults.

sets the values for the global minimum and maximum size, and growth rate.

enables you to apply periodicity to the size field by selecting one source face zone.

Note

Ensure that periodicity is previously defined in the Make Periodic Boundaries

enables you specify the scale factor, and minimum and maximum size values to filter the size

output from the size field.

un-set-periodicity-filter

allows you to use curvature data from the nodes of the CAD facets.

domains/

enters the domain menu.

activate

activates the specified domain for meshing or reporting operations.

create

creates a new domain based on the specified boundary face zones. Ensure valid boundary zones

are specified; specifying invalid zones will generate an error.

create-by-cell-zone

creates a new domain based on the specified cell zone.

mesh/

create-by-point

creates a new domain based on the specified

Note

The create-by-point option works only for cases with no overlapping face zones.

delete

deletes the specified domain.

draw

displays the boundary face zones of the specified domain.

print

prints the information for the specified domain.

hexcore/

enters the hexcore menu.

controls/

enters the hexcore controls menu.

buffer-layers

sets the number of addition cells to mark for subdivision.

compute-max-cell-length

computes the maximum cell length for the hexcore mesh.

define-hexcore-extents?

enables you to extend the hexcore mesh to specified domain extents and/or selected planar

boundaries.When enabled, the outer-domain-params sub-menu will be available.

delete-dead-zones?

toggles the automatic deleting of the dead zones.

island-thresholds

opens a dialog to set absolute-island-count (default is ) and island-volume-frac-

tion (relative to total volume of hex cells, default is 1e-). For a cell region to be interpreted as

an island, both cell count and relative volume thresholds may not be exceeded.

keep-hex-tet-separate?

toggles the merging of Cartesian cells with the tet (and wedge) cells at the end of the hexcore

meshing process.

maximum-cell-length

sets the maximum cell length for the hex cells in the domain.

maximum-initial-cells

specifies the maximum number of cells in the initial Cartesian mesh.

maximum-subdivisions

number of changes in size (hanging node subdivisions) allowed in the hex mesh region.The default

is .

non-fluid-type

selects the default non-fluid cell zone type. After the mesh is initialized, any non-fluid zones will

be set to this type. If the mesh includes multiple regions (for example, the problem for which you

are creating the mesh includes a fluid zone and one or more solid zones), and you plan to refine

all of them using the same refinement parameters, modify the Non-Fluid Type before generating

the hexcore mesh.

Note

For zone-based meshing, if any cell zone has at least one boundary zone type as

inlet, it will automatically be set to fluid type. For object based meshing, volume

region type is used to determine the cell zone type.

octree-hexcore?

speeds up hexahedral core generation by enabling the octree technique for hexcore mesh gener-

ation.This option is disabled by default.

Body-of-influence sizing may be used for refinement.

This option does not support hexcore generation up to boundaries.

only-hexcore?

enables you to create only the hexcore mesh and activates the tetrahedral mesh domain (without

tetrahedral mesh generation). It enables you to prevent the automatic creation of the mesh after

hexcore generation.This option is disabled by default.This option is not available for object-based

meshing.

outer-domain-params/

meshing.

contains options for defining the outer domain parameters.This sub-menu is available only when

define-hexcore-extents? is enabled.

specify-coordinates?

enables you to specify the extents of the hexcore outer box using the coordinates command.

coordinates

specifies the extents (min and max coordinates) of the hexcore outer box.This command is

available when the specify-coordinates? option is enabled.

specify-boundaries?

enables you to specify selected boundaries to which the hexcore mesh is to be generated using

the boundaries command.

specifies the boundaries to which the hexcore mesh is to be generated when the specify-

boundaries? option is enabled. After specifying the boundaries, the auto-align?, de-

lete-old-face-zones?, and list options will also be available.

auto-align?

enables you to axis-align non-aligned planar boundaries to which hexcore mesh is to be gen-

erated.This option is available only when the specify-boundaries? option is enabled

and the boundaries are specified.

mesh/

auto-align-tolerance

specifies the tolerance for aligning boundary zones when auto-align? is enabled.

auto-align-boundaries

aligns the boundary zones specified (using the boundaries command) with the tolerance

specified \ (using the auto-align-tolerance command) when auto-align? is enabled.

delete-old-face-zones?

enables you to delete the original tri face zones that have been replaced during the hexcore

meshing process.This option is available only when the specify-boundaries? option is

enabled and the boundaries are specified.

list

list

lists the boundaries to which the hexcore mesh is to be generated.This option is available only

when the specify-boundaries? option is enabled and the boundaries are specified.

peel-layers

specifies the distance for the hexcore interface to peel-back from the boundary.The default value

is .The higher the value of peel layer, the bigger the distance between the hexcore interface and

the boundary.

skip-tet-refinement?

enables you to omit the tetrahedral refinement phase for reducing total cell count (default is no).

Hex cell count is unaffected.

Tip

It is recommended to use peel-layers equal  when this option is enabled.

Warning

This option may leave narrow regions without hexcore mesh. Tetrahedral cells

with lower quality may be created in such regions, reducing the overall mesh

quality.

smooth-interface?

enables smoothing of the hexcore interface.

smooth-iterations

specifies the number of smoothing iterations.

smooth-relaxation

specifies the surface smoothing relaxation factor.

create

enables you to create the hexcore mesh according to the specified parameters.

enters the hexcore local refinement region sub-menu.

activate

enables you to activate the specified local regions for refinement.

deactivate

enables you to deactivate the specified local regions for refinement.

define

defines the local region according to the specified parameters.

delete

ideal-hex-vol

reports the ideal hex volume for the given edge length.

init

creates a default region encompassing the entire geometry.

lists the defined and active regions in the console.

init

laplace-smooth-nodes

applies a Laplacian smoothing operator to the mesh nodes.This command can be used for smoothing of

all cell types, including prismatic cells.

list-mesh-parameter

shows all mesh parameters.

manage/

enters the manage cell zones menu.

active-list

lists all active zones.

adjacent-face-zones

lists all face zones that refer to the specified cell zone.

auto-set-active

sets the active zones based on points that are defined in an external file. For each zone you want to

activate, you need to specify the coordinates of a point in the zone, the zone type (for example, fluid),

and (optionally) a new name. A sample file is shown below:

((. -. .) fluid heater-#)

((. -. .) fluid below-heater-#)

((. -. .) fluid above-heater-#)

((. -. .) fluid plenum-#)

Here, four fluid zones are identified, renamed, and activated. Any zone that you identify in the

file will automatically be activated. The # indicates that the mesher should append the appro-

priate ID number for the zone.

Warning

This command is valid only for tet meshes.

enables you to change the prefix for the cell zone.

mesh/

copy

copies all nodes and faces of specified cell zones.

delete

deletes a cell zone, along with its associated nodes and faces.

get-material-point

prints the coordinates of the material point for the specified cell zone.

Note

If the cell zone is non-contiguous, the get-material-point command will print

a list of material points, one for each contiguous region.

id

specifies a new cell zone ID. If a conflict is detected, the change will be ignored.

id

list

prints information on all cell zones.

merge

merges two or more cell zones.

Note

For object-based merge, the selected zones must be in the same volumetric region.

If not, you will have to merge the volumetric regions first using /objects/volu-

metric-regions/merge. If the volumetric regions cannot be merged because

they are not contiguous, you will have to delete the object(s) only before merging

the cell zones.

merge-dead-zones

enables you to merge dead zones having a cell count lower than the specified threshold value, with

the adjacent cell zone.The result of the merge operation is determined by the type of the adjacent

cell zone and the shared face area.The priority for merging with the adjacent cell zone based on type

is fluid > solid > dead (that is, merging with an adjacent fluid zone takes priority over merging with

an adjacent solid zone, which in turn takes priority over merging with a dead zone). Also, if the adjacent

zones are of the same type (for example, fluid), the zone will be merged with the zone having the

largest shared face area.

name

enables you to rename a cell zone.

origin

specifies a new origin for the mesh, to be used for cell zone rotation.The default origin is (,,).

revolve-face-zone

generates cells by revolving a face thread.

rotate

rotates all nodes of specified cell zones by a specified angle.

rotates all nodes of the model by a specified angle.

scale

scales all nodes of specified cell zones by a specified factor.

scales all nodes of the model by a specified factor.

set-active

sets the specified cell zones to be active.

scale

translate

translates all nodes of specified cell zones by a specified vector.

translates all nodes of the model by a specified vector.

type

changes the type and name of a cell zone.

modify/

enters the mesh modify menu.

auto-improve-warp

enables you to improve face warp by node movement. Specify the appropriate cell zones and

boundary zones, the maximum warp, the number of iterations per face to be improved, and the

number of iterations of the automatic node movement procedure (default, ).

enables you to improve the mesh quality by node movement. Specify the appropriate cell zones and

boundary zones, the quality limit based on the quality measure selected, dihedral angle, the number

of iterations per node to be moved and the number of iterations of the automatic node movement

procedure (default, ).You can also choose to restrict the movement of boundary nodes along the

surface.

clears all items from the selection list.

deselects the last item you selected using the select-entity command.

extract-unused-nodes

places all unused nodes in a separate interior node zone.

lists all items in the selection list.

list-skewed-cells

lists cells with skewness in a specified range.

mesh-node

attempts to introduce a new node into the existing mesh.

mesh/

mesh-nodes-on-zone

inserts nodes associated with node or face zone into the volume mesh.

Important

If a face zone is specified, the faces are deleted before the nodes are introduced into

the mesh.

neighborhood-skew

Important

the mesh.

reports the maximum skewness of cells using the specified node.

refine-cell

attempts to refine the cells in the probe list by introducing a node nears its centroid.This technique

is useful for removing very flat cells near the boundary when boundary sliver removal is not possible.

After refining the cell, you should smooth the mesh.

repair-negative-volume-cells

repairs negative volume cells by moving nodes. Specify the appropriate boundary zones, the number

of iterations per node to be moved, dihedral angle, whether to restrict the movement of boundary

nodes along the surface, and the number of iterations of the automatic node movement procedure

(default, ).

adds an entity (face, node, cell, etc.) to the selection list.

smooth-node

applies Laplace smoothing to the nodes in the selection list.

enters the non-conformals menu.

controls/

enters the non-conformals controls menu.

enable?

toggles the creation of a non-conformal interface.

retri-method

specifies the method to be used for retriangulating the quad faces on the non-conformal zones.

prism

remeshes the prism-side quad zones named prism-side* or *-quad*.

quad-split

splits the quad faces diagonally into tri faces.

remesh

remeshes all the quad faces based on the edge and surface feature angle specified.

create

creates the non-conformal interface on the specified face zones using the specified retriangulation

method.

separate

enables you to separate the face zones comprising the non-conformal interface between the cell zones

specified. Specify the cell zones where the interface is non-conformal, an appropriate gap distance,

and the critical angle to be used for separating the face zones.You can also choose to orient the

boundary face zones after separation and additionally write a journal file for the separation operation.

Note

If you choose to write a journal file when using the /mesh/non-conformals/sep-

arate command to separate the mesh interface zones, you can read the journal file

to create the mesh interface automatically in solution mode.

poly/

enters the polyhedral mesh generation menu.

collapse

merge nodes to remove short edges and small faces.The decision threshold uses edge size ratio, face

size ratio, and (face) area fraction.

controls/

enters the controls menu for setting poly parameters.

cell-sizing

sets cell volume distribution function as geometric, linear, or size-field.

edge-size-ratio

sets the threshold for the size ratio of two connected edges. Recommended range is  to .

face-size-ratio

sets the threshold for the size ratio of two faces on one cell. Recommended range is  to .

sets the minimum threshold that should be preserved as a feature.

improve?

enables poly mesh improvement by smoothing based on the smooth-controls.

merge-skew

sets the minimum skewness threshold for cell merge.

selects the default type for non-fluid zones.

remesh-skew

sets the target skewness when remeshing.

sliver-cell-area-fraction

sets the threshold for the area of a single face to the cell surface area. Recommended range is

. to ..

smooth-controls/

enters the menu for setting smoothing parameters for poly mesh.

mesh/

centroid-smooth-iterations

. to ..

mesh/

sets the number of passes for tet-cell centroid smoothing during the poly mesh generation

phase.

edge-smooth-iterations

sets the number of passes for tet-cell edge smoothing during the poly mesh generation phase.

laplace-smooth-iterations

sets the number of passes for tet-cell Laplace smoothing during the poly mesh generation

phase.

smooth-attempts

sets the maximum number of movements for a single node during poly mesh smoothing.

smooth-boundary

enables boundary smoothing as part of poly cell smoothing. Default is no.

sets the number of improvement passes over the full poly mesh.

smooth-on-layer

constrains movement of nodes to maintain layering during poly mesh smoothing.

smooth-skew

sets the minimum skewness threshold for poly mesh smoothing.

improve

allows you to improve the polyhedral mesh quality based on the quality-method.

Note

Poly meshing follows tet meshing. These commands behave like the equivalent

commands under /mesh/tet/local-regions/.

activate

activates the specified regions for refinement.

deactivates the specified regions for refinement.

define

delete

ideal-vol

reports the volume of an ideal tetrahedron for the edge length specified.

init

defines the default refinement region encompassing the entire geometry.

lists all refinement region parameters and the activated regions in the console.

refine

init

refine

refines the active cells inside the selected region based on the specified refinement parameters.

quality-method

asks you to choose from internal-default, orthoskew or squish quality measure for mesh

remesh

improves the quality in a local region based on the minimum skewness threshold.

poly-hexcore,

enters the menu for poly-hexcore mesh.

controls

enters the menu for setting parameters for poly-hexcore mesh.

avoid-:-cell-jump-in-hexcore

determines the types of cells (large cells, small cells, or both) that are going to be replaced with

polyhedra cells in order to avoid any : cell jumps in the hexcore region.

mark-core-region-cell-type-as-hex?

determines whether or not to apply hexahedra cells in the core region of the mesh.The default

value is yes.

only-polyhedra-for-selected-regions

determines if polyhedra cells are to be applied to the selected regions.

prepares the mesh for solving in solution mode by performing a cleanup operation after the volume mesh

has been generated. Operations such as deleting dead zones, deleting geometry objects, deleting edge

zones, removing face/cell zone name prefixes and/or suffixes, deleting unused faces and nodes are per-

formed during this operation.

prism/

enters the prism menu.

controls/

enters the prism controls menu.

adjacent-zone/

enters the prism adjacent zone controls menu.

project-adjacent-angle

determines whether or not to project to an adjacent zone. If a zone shares outer nodes with

any of the zones from which the layers are being grown (the “base zones”), its angle with respect

to the growth direction is compared with this value. If the angle is less than or equal to this

value, then the zone will be projected to.The default value is  degrees. See Using Adjacent

Zones as the Sides of Prisms for details.

mesh/

project-converged

sets the convergence criterion for iterative projection.This is non-dimensionalized by the offset

height at each local node.

project-iter

sets the maximum number of iterations to perform when projecting to multiple zones. Most

projections converge in only a few iterations.There is normally no need to change this value.

project?

enables/disables projection of outer nodes to adjacent zones.

retri-feature-angle

enables you to specify the feature angle that should be prevented while generating prisms.

retriangulate-adjacent?

specifies whether or not triangular face zones adjacent to which outer nodes have been pro-

jected, will be automatically retriangulated.

side-feature-align-angle

specifies the angle used for aligning projected normals along a feature edge.

side-feature-angle

specifies the angle used for computing the feature normals.

side-topology-align-angle

specifies the angle used for aligning projected normals along a particular feature edge based

on the topology.This is particularly useful when the side-feature-angle specified is not

sufficient to decide the feature edge to align the projected normals.

auto-separate-cells?

enables/disables automatic separation of the cells extruded from different face zones to different

Note

Note

This option is not considered when the auto-mesh option is used to generate

the mesh.

check-quality?

enables/disables the checking of volume, skewness, and handedness of each new cell and face.

grow-individually?

specifies whether prisms should be grown from multiple zones individually so that the individual

prism cell zones and the individual cap face zones are retained.

improve/

enters the prism smoothing controls menu.

check-allowable-skew?

enables you to check the skewness of the prism cap for every layer.

check-size?

enables the checking of cell size during the generation of each prism layer. An error will be

reported if zero-area prism cells are generated and prism layer growth will be stopped.

When the check-size? option is disabled, the zero-area prism cells generated can be

removed during the improvement smoothing operations performed at the end of the prism

generation procedure.

corner-height-weight?

when enabled, the offset height at corners with large angles (for example, 270º) is reduced to

give a smoother prism cap.

edge-smooth-angle

specifies the maximum allowable angle between the normals of adjacent cap faces for skewness-

driven edge smoothing.

edge-smooth?

enables/disables local smoothing of nodes of the longest edges of skewed faces.This option

is switched off by default.

edge-swap-base-angle

specifies the maximum allowable angle between the normals of the base faces for skewness-

driven edge swapping.

edge-swap-cap-angle

specifies the maximum allowable angle between the normals of the cap faces for skewness-

edge-swap?

enables/disables edge swapping to decrease the skewness of highly skewed faces.This option

face-smooth-converged

specifies the convergence criteria for cap face smoothing.

face-smooth-rings

sets the number of rings around each node to be smoothed. If zero, only a node itself is

smoothed. If one, the node and all of its neighbors are smoothed. If two, the neighbors of the

neighbors are also smoothed, and so on.

face-smooth-skew

specifies the minimum skewness to smooth cap faces.

face-smooth?

enables face-driven smoothing to improve skewness.

identify-feature-line?

enables you to smooth the normal along the feature lines of the base face zones, during normal

smoothing.This option is disabled by default.

improve-warp?

enables or disables improving of face warp during prism generation.This option is disabled

layer-by-layer-smoothing?

enables you to improve cell quality for every layer by smoothing normals in the current layer.

In addition, perturbation smoothing will be performed to improve cell quality in the lower

layer, when the quality measure is set to either skewness, squish, ICEM CFD quality, or orthoskew.

mesh/

The poor quality elements are identified based on the value set for max-allowable-cell-

skew.The cell aspect ratio will also be maintained during the cell quality improvement.This

option is switched off by default.

left-hand-check

controls checking for left-handedness of faces.The default setting of  implies face handedness

will not be checked. A value of  implies only cap faces will be checked, while  implies faces

of all cells in current layer will be checked.

max-allowable-cap-skew

specifies the maximum skewness allowed for a prism cap face. If the skewness of a cap face

exceeds this value, the meshing process will stop and a warning indicates that the skewness

for that layer is too high.

max-allowable-cell-skew

specifies the cell quality criteria for smoothing and quality checking.

node-smooth-angle

refers to the maximum deviation of a node’s sharpest angle (that is, the most acute angle

between adjacent faces that use the node) from  degrees.The node will be smoothed only

if its sharpest angle falls within this range.

node-smooth-converged

sets the convergence criterion for node smoothing. If the node positions are changing by less

than this value, smoothing iterations will stop.

node-smooth-iter

specifies the maximum number of node smoothing iterations to be performed for the nodes

on each layer.These iterations will be performed until the convergence criterion is reached.

node-smooth-local?

enables node smoothing to converge locally.This is useful for large geometries.

node-smooth-rings

controls the locality of node smoothing by setting the number of rings around each node to

be smoothed. If zero, only the node itself is smoothed. If one, the node and all of its neighbors

are smoothed. If two, the neighbors of the neighbors are also smoothed, and so on.

node-smooth?

enables/disables node smoothing to decrease skewness.This option is switched off by default.

post-adjust-height?

enables you to perform prism height adjustment based on growth rate.

shrink-left-handed-cap?

enables shrinking of prism layers to remove left handed faces.

smooth-improve-prism-cells?

enables you to set the parameters for improving the prism cells after the required prism layers

are created.You can select optimized smoothing (smooth), node movement (improve), or

a combination of both to improve the quality. Specify the quality measure to be used, the cell

quality threshold, the number of improvement iterations, and the minimum improvement re-

quired.

swap-smooth-skew

specifies the skewness threshold for edge swapping and edge and node smoothing.The faces

with skewness greater than or equal to the specified value will be swapped and/or smoothed.

merge-ignored-threads?

enables you to automatically merge all ignored zones related to a base thread into a single thread.

This option is enabled by default.When this option is disabled, more than one ignored thread will

be generated per base thread. However, various zones can be created by ignoring this option.

They are:

:dwall

is formed due to dangling wall.

:prox

is formed due to proximity.

:ud_normal

is formed due to invalid normal.

:smooth

is formed due to smoothing of ignored regions.

The default value of the tgvar prism/ignore-extension (for which there is no TUI

command) is . It means that after the prism generation is over, all the ignored regions are

expanded by this number. If we expand say by n times, that is if prism/ignore-exten-

sion is set to n using tgsetvar! (with the exclamation mark), more ignored threads will

be created because of expanding ignored regions. These regions will be named as follows:

:cell_delete_1, *:cell_delete_2, *:cell_delete_3,.... up to \

:cell_delete_n

If merge-ignored-threads? is enabled, then all these are merged and you finally get

only one zone per base thread, named as *:ignore.

morph/

enters the prism morphing controls menu.

improve-threshold

specifies the quality threshold used for improving the quality during the morphing operation.

morphing-convergence-limit

specifies the convergence limit for the morphing operation.The morpher uses an iterative

solver. It is assumed to have converged when the relative residual is less than this number.

morphing-frequency

specifies the frequency of the morphing operation.The number specified denotes the number

of prism layers after which the morpher is applied to the remainder of the mesh (for example,

a value of  indicates that the morpher is applied to the mesh after every  prism layers grown).

normal/

enters the prism normal controls menu.

mesh/

bisect-angle

is required for growing prisms out of sharp interior corners.When the value of this angle is set,

the normals are automatically projected onto the plane bisecting the angle between faces

having an interior angle less than this angle.

compute-normal

computes the normal for the specified face zone.

converge-locally?

specifies whether or not the normal smoothing at each node is frozen once convergence is

satisfied at that node. If not, all normals are continuously smoothed until all of them have

direction-method

specifies whether the prism layers should be grown normal to surfaces or along a specified

direction vector.

direction-vector

specifies the direction vector for prism extrusion when the uniform method is selected for

direction-method.

ignore-invalid-normals?

enables you to ignore nodes that have poor normals.

max-angle-change

specifies the maximum angle by which the normal direction at a node can change during

normal-method

gives options for the method to use for computing the normal direction.

acute-bisection

is a variation of that proposed by Kallinderis et al. [], [].The faces surrounding a node are

analyzed to find those whose planes form the most acute angle.The resulting normal lies

on the plane bisecting those two planes.

This method is computationally more expensive than surface averaging, but is less

robust at singular points where convex edges meet smooth surfaces. For example,

if a box is sitting on the table, such a point would be where one of the box’s corners

meets the table top.

face-average

computes the normal at a node by averaging the normals of the surrounding faces.

hybrid-normal

computes the normal by all the methods available and uses the best quality normal ob-

tained.This is the default method.

minimized-angle

is a variation of that proposed by Pirzadeh [], []. An ial normal at a node is determined

by averaging the normals of the surrounding faces (the face-average method). Iterations

are then performed to minimize the largest angle between the node normal and the normals

of the surrounding faces.

This method is a computationally more expensive than surface averaging, and can

produce slightly better normals when the uniform offset method is used and the

surface mesh does not contain sharp edges. When the minimum-height offset

method is used, this direction method may introduce spikes and pits in the advancing

layer surfaces.

surface-average

is similar to face-average, but handles sharp edges better.

orient-mesh-object-face-normals

enables you to orient the face normals for mesh object boundary zones. Specify the mesh object,

region or material point as appropriate, and specify whether walls, baffles or both comprising

the prism base zones are to be separated and oriented.

orthogonal-layers

specifies the number of layers to preserve orthogonality. All smoothing is deferred until after

these layers.

smooth-converged

sets the convergence criterion (in degrees) for normal smoothing. If the normal directions are

changing by less than this value, smoothing iterations will stop.

smooth-iter

specifies the maximum number of normal smoothing iterations to be performed for the normal

vectors on each layer.These iterations will be performed until the convergence criterion

(normal/smooth-converged) is reached.

smooth?

enables or disables smoothing of normal direction vectors.

offset/

enters the prism offset controls menu.

first-aspect-ratio-min

specifies the minimum first aspect ratio (ratio of prism base length to prism layer height) for

the prism cells.

min-aspect-ratio

specifies the minimum aspect ratio (ratio of prism base length to prism layer height) for the

prism cells.

sets the convergence criterion for offset smoothing. If the offset heights are changing by less

sets the maximum number of offset smoothing iterations to be performed.These iterations

will be performed until the convergence criterion offset/smooth-converged is reached.

smooth?

enables/disables offset distance smoothing.

mesh/

post-ignore/

contains options for setting the parameters for removing poor quality prism cells after the required

prism layers are created.

post-remove-cells?

enables you to set the parameters for removing poor quality prism cells after the required

prism layers are created.You can remove cells based on quality, intersection, interior warp,

and feature edges. Specify options for removing additional cells in regions of high aspect ratio

and feature angle, the number of cell rings to be removed around the marked cells, and options

for smoothing the prism boundary and prism side height.

proximity

enters the prism proximity controls menu.

allow-ignore?

enables you to ignore nodes where the specified maximum shrink factor cannot be maintained.

allow-shrinkage?

enables shrinkage while growing prism layers.

gap-factor

controls the gap between the intersecting prisms layers in the proximity region with respect

to the cell size of the prisms.

keep-first-layer-offsets?

enables you to retain first layer offsets while performing proximity detection.

max-aspect-ratio

specifies the maximum allowable cell aspect ratio to determine the limit for the shrinkage of

prism layers.This option is available only when the allow-ignore? option is disabled.

max-shrink-factor

specifies the shrink factor determining the maximum shrinkage of the prism layers.This option

is available only when the allow-ignore? option is enabled.

smoothing-rate

specifies the rate at which shrinkage is propagated in lateral direction.

remove-invalid-layer?

removes the last prism layer if it fails in the quality check.

set-post-mesh-controls

sets controls specific to growing prisms post volume mesh generation.

split?

enables you to set parameters for splitting the prism layers after the initial prism layers are gener-

ated, to generate the total number of layers required. Specify the number of divisions per layer.

zone-specific-growth

enters the prism growth controls menu.

apply-growth

applies the zone-specific growth parameters specified.

clear-growth

clears the zone-specific growth specified.

list-growth

lists the zone-specific growth parameters specified for individual zones in the console.

create

creates prism layers on one or more boundary face zones based on the offset method, growth method,

number of layers, and rate specified.

improve/

enters the prism improve menu.

improve-prism-cells

collects and smooths cells in layers around poor quality cells. Cells with quality worse than the

specified threshold value will be identified, and the nodes of the cells surrounding the poor quality

cells will be moved to improve quality.

smooth-brute-force?

forcibly smooths cells if cell skewness is still high after regular smoothing.

smooth-cell-rings

specifies the number of cell rings around the skewed cell used by improve-prism-cells.

smooth-improve-prism-cells

uses a combination of node movement and optimized smoothing to improve the quality.This

command is a combination of the smooth-prism-cells and improve-prism-cells

commands.The cell aspect ratio will also be maintained based on the value specified for max-

smooth-prism-cells

enables optimization based smoothing of prism cells.The nodes of cells with quality worse than

the specified threshold value will be moved to improve quality.The cell aspect ratio will also be

maintained based on the value specified for max-aspect-ratio.

smooth-sliver-skew

specifies the skewness above which prism cells will be smoothed.

list-parameters

shows all prism mesh parameters.

mark-ignore-faces

enables you to mark the faces to be ignored during prism meshing.

mark-nonmanifold-nodes

enables you to mark the non-manifold prism base nodes. A list of the non-manifold nodes will be

printed in the console.The faces connected to the non-manifold nodes will also be marked.You can

use this command after specifying zone-specific prism settings, prior to generating the prisms to

verify that non-manifold configurations do not exist.

contains the following options for ignoring prism cells:

mesh/

create-cavity

creates a cavity in regions where prism quality is adequate, but the quality of adjacent tetrahedra

is poor.The cavity is created based on the tetrahedral cell zone, the quality measure and the cor-

responding threshold value, and the additional number of cell rings specified.You can create a

cavity comprising only tetrahedral cells or optionally include prism cells in the cavity created.When

prism cells are also included in the cavity, you can specify whether the non-conformal interface is

to be created.

mark-cavity-prism-cap

marks the prism cap faces and tetrahedral cell faces bounding the cavity to be created in regions

where prism quality is adequate, but the quality of adjacent tetrahedra is poor. Specify the tetra-

hedral cell zone, the quality measure and the corresponding threshold value to be used, and the

additional number of cell rings based on which the cavity will be created.

mark-prism-cap

marks the prism cap faces for ignoring prism cells in regions of poor quality cells and sharp corners.

Specify the prism cell zone and the basis for ignoring prism cells and the relevant parameters.The

prism cells can be ignored based on quality, intersection, (both enabled by default), warp, and

features (both disabled by default). Specify the quality measure and threshold value to be used

for ignoring cells based on quality and (if applicable) the feature edges for ignoring cells based on

features. Additionally, specify whether cells are to be marked in regions of high aspect ratio and

based on feature angle, and the additional number of cell rings based on which prism cells will be

removed.

post-remove-cells

enables you to remove prism cells in layers around poor quality cells and sharp corners. Specify

the prism cell zone, the basis for ignoring prism cells (quality, intersection, warp, features) and the

relevant parameters. Specify the number of cell rings to be removed around the marked cells. Cells

will be marked for removal in regions of sharp corners based on quality, intersection, warp, and

features (as applicable) and then extended based on the number of cell rings specified. Additional

cells will be marked for removal in regions of high aspect ratio and based on feature angle (if ap-

plicable) around the exposed prism side.The boundary will be smoothed at feature corners after

the prism cells have been removed.The prism-side faces exposed by the removal of the prism cells

will be collected in a zone named prism-side-#, while for a zone wall-n, the faces correspond-

ing to the ignored prism cells will be collected in a zone named wall-n:ignore.You can also

optionally smooth the prism side nodes from the base node to the cap node to create better tri-

angles for the non-conformal interface.

specifies the quality method used during prism generation.

reset-parameters

resets all prism parameters.

split/

contains options for splitting the prism layers after the initial prism layers are generated, to generate

the total number of layers required.

split

enables you to split the prism layers after the initial prism layers are generated, to generate the

total number of layers required. Specify the prism cell zones to be split and the number of divisions

per layer.You can also choose to use the existing growth rate (default) or specify the growth rate

to be used while splitting the prism layers.

pyramid/

enters the pyramid menu.

controls/

enters the pyramid controls menu.

neighbor-angle

pyramid/

controls/

sets the threshold dihedral angle used to limit the neighboring faces considered for pyramid cre-

ation. For example, if the value is set to ° and the angle between a given quadrilateral face and

a neighboring triangular face is greater than °, the resulting pyramid will not include the trian-

gular face.

offset-factor

specifies the fraction of the computed pyramid height (offset) by which the pyramid heights will

be randomly adjusted.The default value is , indicating that all pyramids will have the exact height

computed. A value of ., for example, will limit each adjustment to ±% of the computed height.

offset-scaling

specifies the scaling, to be used to determine the height of the pyramid.

vertex-method

specifies the method by which the location of the new vertex of the pyramid will be determined.

The skewness method is used by default.

create

creates a layer of pyramids on the quad face zone.

repair-face-handedness

reverses face node orientation.

reset-mesh

clears the entire mesh.

reset-mesh-parameter

resets all parameters to their default value.

contains options for creating scoped prism controls for mesh objects.

create

creates a new scoped prism control based on the parameters and scope specified. Specify the name,

offset method, first height or aspect ratio, number of layers, and rate or last percent. Select the mesh

object and set the scope (fluid-regions, named-regions, or solid-regions). Specify the

zones to grow prisms (all-zones, only-walls, selected-face-zones, or selected-labels,

or solid-fluid-interface).When named-regions and/or selected-face-zones or

selected-labels are selected, specify the volume and/or boundary scope. If interior baffle zones

are selected, retain the option to grow prisms on both sides of the baffles or disable it to grow prisms

on one side.

delete

deletes the specified scoped prism control.

mesh/

growth-options

enables you to specify scoped prism growth options. Select Fix First Height if required, and

specify the gap factor, maximum aspect ratio, prism quality method, and the threshold quality value

for stair stepping.

list

lists all the defined scoped prism controls.

modify

modifies the specified control based on the parameters specified.

read

reads in the specified scoped prism control file (*.pzmcontrol).

set-no-imprint-zones

used to specify face zones that should not be imprinted during prism generation.

write

writes the scoped prism controls to a prism control file (*.pzmcontrol). Specify the scoped prism file

name.

selective-mesh-check

performs a customized mesh check on specific zones rather than all zones.

separate

separates cells by various user-defined methods.

define

enables you to define the parameters for the refinement region.

delete

enables you to delete a refinement region.

init

deletes all current regions and adds the default refinement region.

lists all the refinement regions.

separate-cell-by-face

separates cells that are connected to a specified face zone into another cell zone.This separation

method applies only to prism cells.

separate-cell-by-mark

separates cells within a specified local region into another cell zone.

separate-cell-by-region

separates contiguous regions within a cell zone into separate cell zones.

separate-cell-by-shape

separates cells with different shapes (pyramids, tetrahedra, etc.) into separate cell zones.

separate-cell-by-size

separates cells based on the specified minimum and maximum cell sizes.

separate-cell-by-skew

separates cells based on the specified cell skewness.

tet/

enters the tetrahedral mesh menu.

controls/

enters the tet controls menu.

adv-front-method

enters the advancing front refinement controls menu.

first-improve-params

defines the refining front improvement parameters for the advancing front method.

refine-parameters

defines the cell zone improvement parameters for the advancing front method.

second-improve-params

skew-improve/

enters the refine improve controls menu.

attempts

specifies the number of overall improvement attempts for the advancing front method.

boundary-sliver-skew

specifies the boundary sliver skewness for the advancing front method.This parameter is

used for removing sliver cells along the boundary.

iterations

specifies the number of improvement iterations in each attempt for the advancing front

method.

sliver-skew

specifies the sliver skewness for the advancing front method.This parameter is used for

removing sliver cells in the interior.

target-low-skew

specifies the targeted skewness threshold above which cells will be improved.The improve

operation will attempt to improve cells with skewness above the target-low-skew

value specified, but there will be no attempt to reduce the skewness below the specified

value. A limited set of improve operations will be used as compared to the operations re-

quired for the target-skew value-based improvement.The value specified could be

approximately . lower than the target-skew value.

target-skew

specifies the targeted skewness during improvement for the advancing front method.

mesh/

target?

enables you to enable targeted skewness-based refinement for the advancing front

method.This option enables you to improve the mesh until the targeted skewness value

is achieved.

advanced/

enters the advanced tet controls menu.

defaults?

enables/disables the use of the default values for the initialization parameters.

freeze-boundary-cells

freezes the boundary cells during mesh improvement and sliver removal operations.

keep-virtual-entities?

enables/disables the automatic deleting of virtual entities after mesh initialization.

max-cells

sets the maximum number of cells in the mesh.

max-nodes

sets the maximum number of nodes in the mesh.

Warning

Be careful when you set upper limits on the number of cells or nodes. Nodes

or cells will not be added when the prescribed limit is reached, and this may

leave the mesh unevenly refined and less than adequate.

node-tolerance

defines the smallest distance between two distinct nodes.This command is available only

when you disable the use of default values for the initialization parameters.

progress-reports

enables you to set the time between progress reports in seconds.

report-max-unmeshed

reports the maximum number of unmeshed entities.

report-unmeshed-faces?

reports the unmeshed faces.

report-unmeshed-nodes?

reports the unmeshed nodes.

sliver-size

is the smallest cell whose size can be determined accurately.This command is available only

specifies the cell sizing function for refinement.You can select geometric, linear, none, or

size-field as appropriate.

compute-max-cell-volume

computes the maximum cell volume for the current mesh.

specifies the maximum allowable cell volume.

delete-unused-nodes?

toggles the deleting of unused nodes during mesh initialization.

improve-mesh/

enters the improve mesh controls menu.

improve?

automatically improves the mesh.

laplace-smooth

enables you to specify the Laplace smoothing parameters.

skewness-smooth

enables you to specify the skewness smooth parameters.

swap

enables you to specify the face swap parameters.

improve-surface-mesh?

enables you to improve the surface mesh by swapping face edges where Delaunay violations occur.

max-cell-length

specifies the maximum allowable cell length.

max-cell-volume

merge-free-nodes?

enables/disables the merging of free nodes during mesh initialization.

selects the non-fluid cell zone type. After the mesh is initialized, any non-fluid zones will be set to

this type. If the mesh includes multiple regions (for example, the problem for which you are creating

the mesh includes a fluid zone and one or more solid zones), and you plan to refine all of them

using the same refinement parameters, modify the non-fluid type before generating the mesh.

Note

refine-levels

sets the number of refinement levels.

refine-method

enables you to select the refinement method.You can select either skewness-based refinement

or the advancing front method.

mesh/

remove-slivers/

enters the sliver remove controls menu.

angle

specifies the maximum dihedral angle for considering the cell to be a sliver

attempts

specifies the number of attempts overall to remove slivers.

specifies the number of iterations to be performed for the specific sliver removal operation.

low-skew

operation will attempt to improve cells with skewness above the low-skew value specified,

but there will be no attempt to reduce the skewness below the specified value. A limited set

of improve operations will be used as compared to the operations required for the skew value-

based improvement.

method

enables you to select the method for sliver removal.The default method used is the fast

method

method.The fast and the aggressive methods use the same controls and give similar

results for good quality surface meshes. In case of poor surface meshes, the aggressive

method will typically succeed in improving the mesh to a greater extent, but it may be slower

than the fast method.

remove?

enables/disables the automatic removal of slivers.

skew

specifies the skewness threshold for sliver removal.

skewness-method/

enters the skewness refinement controls menu.

levels

specifies the number of refinement levels for skewness-based refinement.

max-skew-improve?

enables/disables the skewness-based improvement during refinement.

must-improve-skewness?

enables/disables the modification of the default auto refinement parameters in order to improve

skewness after refinement.

refine-boundary-cells?

enables/disables the automatic refinement of boundary cells during refinement.

refine-cells?

enables/disables the automatic refinement of cells during refinement.

contains options for improving refinement by the skewness method.This sub-menu is available

when max-skew-improve? is enabled.

attempts

specifies the number of overall improvement attempts for the skewness method.

specifies the boundary sliver skewness for the skewness method.This parameter is used

for removing sliver cells along the boundary.

specifies the number of improvement iterations in each attempt for the skewness method.

specifies the sliver skewness for the skewness method.This parameter is used for removing

sliver cells in the interior.

specifies the targeted skewness during improvement for the skewness method.

target?

enables you to enable targeted skewness-based refinement for the skewness method.This

enables you to improve the mesh until the targeted skewness value is achieved.

smooth-mesh?

enables/disables the automatic smoothing of the mesh during refinement.

sort-boundary-faces?

enables/disables the automatic sorting of boundary faces by size during refinement.

sort-cells?

enables/disables the automatic reverse sorting of cells by skewness during refinement.

swap-faces?

enables/disables the automatic swapping of faces during refinement.

type

enables you to select the appropriate pre-defined skewness refinement parameters.You can

select default, fast-transition, or incremental-improve as required.

use-max-cell-size?

enables you to use the maximum cell size specified instead of recomputing the value based on

the objects, when the volume mesh is generated.This option is disabled by default.

delete-virtual-cells

deletes virtual cells created due to the use of the keep-virtual-entities? option.

improve/

enters the tet improve menu.

mesh/

improve/

mesh/

collapse-slivers

attempts to collapse the nodes of a skewed sliver cell on any one of its neighbors.

improve-cells

improves skewed tetrahedral cells.

refine-boundary-slivers

attempts to increase the volume of boundary slivers to create a valid tet cell.Tetrahedra having

one or two faces on the boundary are identified and then the appropriate edge split.The split

node is then smoothed such that the volume of the tetrahedron increases, thereby creating a valid

tet cell.

refine-slivers

attempts to remove the sliver by placing a node at or near the centroid of the sliver cell. Swapping

and smoothing are performed to improve the skewness.You can also specify whether boundary

cells are to be refined. Refining the boundary cells may enable you to carry out further improvement

options such as smoothing, swapping, and collapsing slivers.

skew-smooth-nodes

applies skewness-based smoothing to nodes on the tetrahedral cell zones to improve the mesh

quality.

sliver-boundary-swap

removes boundary slivers by moving the boundary to exclude the cells from the zone.

smooth-boundary-sliver

smooths nodes on sliver cells having all four nodes on the boundary until the skewness value is

less than the specified value.The default values for the skewness threshold, minimum dihedral

angle between boundary faces, and feature angle are ., , and , respectively.

smooth-interior-sliver

smooths non-boundary nodes on sliver cells having skewness greater than the specified threshold

value.The default value for the skewness threshold is ..

smooth-nodes

enables you to apply either Laplacian or variational smoothing to nodes on the tetrahedral cell

zones to improve the mesh quality.

swap-faces

performs interior face swapping to improve cell skewness.

init

generates the initial Delaunay mesh by meshing the boundary nodes.

init-refine

generates the tetrahedral mesh.

activate

define

delete

ideal-vol

init

refine

preserve-cell-zone

allows you to specify the cell zones to be preserved during the meshing process.

refine

refines the initialized mesh.

trace-path-between-cells

detects holes in the geometry by tracing the path between the two specified cells

thin-volume-mesh/

creates a sweep-like mesh for a body occupying a thin gap.You define source and target boundary faces

zones (the source face normal should point to the target).The source face mesh may be triangles or quads.

create

initiates the dialog box to specify source and target faces and specify the following parameters

Gap Thickness

create

helps Fluent Mesher determine the region to be remeshed. If set to , the mesher will automatically

calculate the gap thickness. If non-zero, the Gap Thickness defines the maximum separation

between source and target zones in the swept-mesh region (default = ).

Number of Divisions

specifies the number of layers created between source and target faces (default = ).

specifies the maximum thickness ratio between two adjacent layers (default = ).

Remesh Overlap Zones

if yes, any overlapped part of the surface mesh on the target and adjacent faces will be remeshed.

Original meshes are replaced (default = yes).

An example create dialog box:

Meshing/mesh/thin-volume-mesh/create

mesh/

()

Source face zones() [()] source*

Source face zones() [()]

()

Target face zones() [()] target

Target face zones() [()]

Gap Thickness []

Number of Divisions []

Growth Rate []

Remesh Overlap Zones? [yes]

Start thin-gap mesh:

Create and project nodes and faces on targets …

Project nodes on targets ...

Create layer nodes ...

Create side quad faces ...

Create interior layer cells ...

Retriangluate target face zones ...

Retriangulate adjacent face zones ...

Done

Chapter : objects/

cad-association/

contains options for modifying the selected objects based on the associated CAD entities and attaching/de-

taching the CAD entities from the objects.This menu is available when the CAD Assemblies tree is created

during CAD import.

attach-cad

attaches CAD entities to the selected geometry/mesh objects. Select the geometry/mesh objects and

specify the path for the CAD entities to be associated with the objects.The selected geometry/mesh

objects will be associated with the CAD entities which will then be locked.

detach-all-objects

detaches all the CAD objects associated with the geometry/mesh objects. Specify the type of objects

(geom or mesh) to be detached. All association will be removed and the geometry/mesh objects will

be independent of changes to the CAD entities.

detach-objects

detaches the CAD objects associated with the specified geometry/mesh objects. All association will

be removed and the selected geometry/mesh objects will be independent of changes to the CAD en-

tities.

query-object-association

returns a list of the CAD entities associated with the objects selected.

restore-cad

restores the geometry/mesh objects from the associated CAD objects.

unlock-cad

unlocks the CAD objects associated with the selected geometry/mesh objects.

update-objects

updates the specified geometry/mesh objects based on changes to the associated CAD objects.

update-all-objects

updates all geometry/mesh objects based on changes to the associated CAD objects. Specify the type

of objects (geom or mesh) to be updated.

allows you to change the object type (geom, or mesh).

checks the mesh on the specified objects for connectivity and orientation of faces.The domain extents,

volume statistics, and face area statistics will be reported along with the results of other checks on the

mesh.

create

creates the object based on the priority, cell zone type, face zone(s), edge zone(s), and object type specified.

mesh.

create

You can specify the object name or retain the default blank entry to have the object name generated

automatically.

creates and activates the domain comprising the face zone(s) from the object(s) specified.

creates a face group and an edge group comprising the face zone(s) and edge zone(s) included in the

specified object(s), respectively.

allows you to create intersection loops for objects.

The collectively option creates an interior edge loop at the intersection between two adjacent

face zones included in the same object and between multiple objects.

The individually option creates an interior edge loop at the intersection between two adjacent

face zones included in the same object.

creates multiple objects by creating an object per face zone specified.The objects will be named automat-

ically based on the prefix and priority specified.

remesh

wrap

delete

deletes the specified object(s).

extracts the edge zone(s) from the face zone(s) included in the specified object(s), based on the edge-

feature-angle value specified (/objects/set/set-edge-feature-angle).

objects/

enables you to imprint the edges comprising the object on to the object face zones to improve feature

capture for mesh objects.You can specify the number of imprinting iterations to be performed.

Note

The geometry objects used to create the mesh objects should be available when the

improve-feature-capture command is invoked. Additionally, the face zones

comprising the objects should be of type other than geometry.

enables you to improve the surface mesh quality for mesh objects. Select the mesh objects and the

method for improving the surface mesh.The smooth-and-improve method improves the mesh by a

combination of smoothing, swapping, and surface mesh improvement operations. Object normals are

correctly oriented and island faces are also deleted.You can optionally coarsen the surface mesh by spe-

cifying a suitable coarsening factor. Additional imprinting operations can be done to improve feature

capture on the surface mesh.The surface-remesh method improves the mesh by remeshing based

on the current size field. Object normals are correctly oriented and island faces are also deleted.

contains options for connecting overlapping and intersecting face zones.

add-objects-to-mesh-object

allows you to specify one or more mesh objects to be added to an existing mesh object.

change-region-type

allows you to select a cell zone type (solid, fluid or dead) for a specific region.

compute-regions

closed cell zone regions are computed from the specified mesh object.You may include a material

point, if desired.

controls/

used to enable or disable automatic post-remesh operation after join or intersect.

create-mesh-object

allows you to specify one or more mesh objects to be connected in one mesh object.

delete-region

removes a closed cell zone region and all of its face zones, except those which are shared by other

regions, from the specified mesh object.

intersect

connects two intersecting face zones within specified angle and tolerance.

join

connects two overlapping face zones within specified angle and tolerance.

lists details of region type, volume, material point, and comprising face zones for the topological regions

computed for the specified mesh object.

specified regions are joined into a single region.

rename-region

enables you to specify a new name for a specified region.

labels/

contains options for creating and managing face zone labels.

add-zones

adds the specified face zones to the existing face zone label for an object.

create

creates a new face zone label for the specified face zones.

create-label-per-object

creates a new face zone label for all the face zones in every object.

create-label-per-zone

creates a new face zone label for each face zone in the object.

delete

deletes the specified face zone labels.

label-unlabeled-zones

creates labels for unlabeled face zones within the specified object.You can either use the object name

as the label or provide your own label.

merge

merge

merges the specified face zone labels to a single label with the name specified.

remove-all-labels-on-zones

removes all the face zone labels for the specified face zones.This command is applicable to geometry

objects only.

removes the specified face zones from the existing face zone label for an object.

rename

renames the specified face zone label.

list

lists details such as cell zone type, priority, object type, comprising face and edge zones, and object reference

point for all the defined objects.

merge

objects/

Note

If the object is composed of edge zones of different types (boundary and interior), the

edge zones of the same type (boundary or interior) will be merged into a single edge

zone.

merges the free nodes at the object level based on the specified tolerance or using a tolerance that is a

specified percentage of shortest connected edge length.

allows you to merge voids in the mesh object after the sewing operation.

contains options for removing gaps between the mesh objects specified or removing the thickness in the

mesh objects specified.

ignore-orientation?

allows you to set whether the orientation of the normals should be taken into account while identifying

the gap to be removed.

remove-gaps

allows you to remove gaps between the mesh objects specified or remove the thickness in the mesh

objects specified. Select the appropriate repair option and specify the other parameters required.

show-gaps

marks the faces at the gap between mesh objects based on the gap distance and percentage margin

rename-cell-zone-boundaries-using-labels

renames the boundaries of the cell zones based on the existing face zone labels.This allows for the cell

zone boundaries in solution mode to have names corresponding to the face zone labels in meshing mode.

Note

This command will not work if you read in a volume mesh generated in a version prior

to release .. In such cases, regenerate the volume mesh before using the command.

, rename-object

allows you to rename a specified geometry or mesh object with another specified name.

renames the face and edge zones comprising the object based on the object name.You can also specify

the separator to be used.

restore-faces

restores the mesh object surface mesh from the backup created.The current mesh object face zones and

If the object backup is disabled (/mesh/auto-mesh-controls/backup-object no), you

will not be able to restore the surface mesh using this command.

Note

There may be a difference in the initial volume mesh generated for an object and that

generated after restoring the object surface mesh due to differences in the order of

zones/entities processed during volume meshing.

rotate

rotates the object(s) based on the angle of rotation, pivot point, and axis of rotation specified.

scale

scales the object(s) based on the scale factors specified.

rotate

scale

separates the face zone(s) comprising the object based on the angle specified.

separates the face zone(s) comprising the object based on the seed face specified.

set/

contains options for setting additional object-related settings.

sets the edge feature angle to be used for extracting edge zone(s) from the face zone(s) included in

the object(s).

displays the edge zone(s) comprising the object(s) drawn in the graphics window.

displays the face zone(s) comprising the object(s) drawn in the graphics window.

sew/

contains options related to the object sewing operation.

Note

sew

connects the mesh objects to generate the conformal surface mesh.

set/

contains additional options related to the object sewing operation.

include-thin-cut-edges-and-faces

allows better recovery of thin region configurations during the sewing operation.

objects/

process-slits-as-baffles?

allows you to collapse the nearly overlapping surfaces corresponding to the baffle when the sew

operation is performed to create the mesh object. Specify the maximum slit thickness relative to

the minimum size specified and the parallel face angle between the faces comprising the slit when

process-slits-as-baffles is enabled.

zone-name-prefix

allows you to specify a prefix for the zones included in the mesh object created using the sew op-

eration.

, summary

eration.

, summary

allows you to obtain a summary of a specified geometry or mesh object, or obtain a summary of all geometry

or mesh objects.

translate

translates the object(s) based on the translation offsets specified.

update

allows you to update the objects defined when the face and/or edge zone(s) comprising the object have

been deleted.

volumetric-regions/

contains options for manipulating volumetric regions and generating the volume mesh.

auto-fill-volume

creates the volume mesh for the selected volumetric regions based on the meshing parameters set.

change-type

enables you to change the region type.

compute

computes the volumetric regions based on the face zone labels.You can choose to use existing mater-

ial points for computing the regions.

Note

labels of the mesh object selected. If regions are recomputed, all previous region

names and types will be over written.

delete

deletes the specified volumetric regions.

Tip

Deleting regions may cause face zones to be deleted. It is recommended that the

region type be changed to dead instead of deleting the region.

delete-cells

deletes the cell zones of the specified regions.

hexcore/

contains options for setting hexcore mesh controls.

list

prints region information to the console, including type, volume, material point and face zones.

merge

merges specified regions in to a single region.

Note

If there are shared face zones, merging regions will delete the shared face zones.

merge

Note

However, if there are cell zones associated with the regions, then merging the regions

will not delete the shared face zones. In this case, the shared face zones will be deleted

when the cell zones are deleted.

rename

renames the region.

scoped-prism/

contains options for setting scoped prism controls.

tet/

contains options for setting tetrahedral mesh controls.

update

recomputes the selected volumetric region(s) while preserving the region name(s) and type(s).

wrap/

contains options related to the object wrapping operation.

check-holes

allows you to check for holes in the objects.The number of hole faces marked will be reported.

allows you to reestablish the periodic relationship between master and shadow face zones on the

mesh object.You will be prompted for the method and to identify the periodic face zones to be re-

covered.

auto

performs the automatic periodic recovery method using either the master or shadow periodic face

zones. Periodic recovery will be attempted in both directions without additional prompting.

manual

performs the manual periodic recovery method.You will be prompted for periodic and shadow

face zones, and for the periodic source.The periodic source may be from an underlying periodic

geometry surface or manual entry of the rotational periodic parameters (angle, origin, axis).

Note

set/

contains additional options related to the object wrapping operation.

objects/

add-geometry-recovery-level-to-zones

set/

objects/

enables you to set the geometry recovery level (high or low) for the specified face zones.

allows better recovery of thin region configurations during the object wrapping operation.

list-zones-geometry-recovery-levels

lists the zones based on geometry recovery level specified.

max-free-edges-for-hole-patching

allows you to set the maximum number of free edges in a loop to fill the holes.

minimum-relative-topo-area

specifies the minimum relative topological area for shrink wrapping.

minimum-relative-topo-count

specifies the minimum relative topological count for shrink wrapping.

minimum-topo-area

specifies the minimum topological area for shrink wrapping.

minimum-topo-count

specifies the minimum topological count for shrink wrapping.

relative-feature-tolerance

specifies the relative feature tolerance for shrink wrapping.

report-holes?

allows you to check for holes in the mesh object created. Holes, if any will be reported at the end

of the object wrapping operation.

resolution-factor

sets the resolution factor for shrink wrapping.This option can be used to set sampling coarser or

finer than the final surface mesh.

shrink-wrap-rezone-parameters

allows you to set the parameters for improving the mesh object surface quality using rezoning.

The geometry object zones will be separated based on the separation angle specified to improve

the feature imprinting on the mesh object.

allows you to specify a prefix for the zones included in the mesh object created using the object

wrap

wrap

creates the mesh objects based on the geometry objects selected and other object wrapping parameters

Chapter : parallel/

agglomerate

recombines distributed mesh data into a single partition on compute node .

auto-partition?

automatically partitions face-zones for parallel meshing.

distribute

allocates mesh to the compute nodes based on the computed partitions.

print-partition-info

displays computed partition data to the console.

spawn-solver-processes

specifies the number of solver processes. Additional processes will be spawned as necessary when

switching to solution mode.You will also be prompted for (Linux and mixed Windows/Linux) interconnect

type, machine list or host file, and (Linux and mixed Windows/Linux) option to be used.

thread-number-control

controls the maximum number of threads on each machine.

Chapter : report/

boundary-cell-quality

reports the number and quality limits of boundary cells containing the specified number of boundary

faces. If you specify zero for number of boundary faces, you will be prompted for number of

boundary nodes.

reports the distribution of cell quality or size based on the bounding limits and number of partitions spe-

cified.

cell-quality-limits

reports the cell quality limits.

cell-size-limits

reports the cell size limits.

cell-zone-at-location

returns the cell zone at or closest to the specified location.

cell-zone-volume

reports the volume of the specified cell zone.

reports the edge size limits.

reports the distribution of face quality or size based on the bounding limits and number of partitions

face-node-degree-distribution

reports the distribution of boundary faces based on face node degree.The node degree is the number of

faces connected to the node. Specify the list of boundary face zones and the minimum and maximum face

node degree to be reported.You can also consider only internal nodes, if required.

face-quality-limits

reports the face quality limits.

face-size-limits

reports the face size limits.

face-zone-area

reports the area of the specified face zone.

face-zone-at-location

reports the face zone at the given location.

list-cell-quality

reports a list of cells with the specified quality measure within a specified range.The valid prefixes are bn

(boundary node), n (node), bf (boundary face), f (face), and c (cell).

memory-usage

reports the amount of memory used for all nodes, faces, and cells, and the total memory allocated.

mesh-size

reports the number of nodes, faces, and cells in the mesh.

mesh-statistics

writes mesh statistics (such as zone information, number of cells, faces, and nodes, range of quality and

size) to an external file.

neighborhood-quality

reports the maximum skewness, aspect ratio, or size change of all cells using a specified node.

number-meshed

reports the number of elements that have been meshed.

prints information about individual components of the mesh.This command also appears in the boundary

menu.When you use this command, you will be prompted for an “entity” (that is, a node, face, or cell). An

entity name consists of a prefix and an index. For a description of the displayed information see Reporting

Mesh Information in the Fluent User's Guide

specifies the method to be used for reporting face and cell quality.

unrefined-cells

reports the number of cells that have not been refined.

update-bounding-box

updates the bounding box.

verbosity-level

specifies how much information should be displayed during mesh initialization, refinement and other

operations. Changing the value to  from the default value of  will produce more messages, while changing

it to  will disable all messages.

report/

Chapter : scoped-sizing/

compute

computes the size field based on the defined size functions and/or scoped size controls.

create

defines the scoped size based on the specified parameters.

delete

deletes the specified scoped size controls.

deletes all the defined scoped size controls.

delete-size-field

deletes the current size field.

list

lists all the defined scoped size controls and the corresponding parameter values defined.

list-zones-uncovered-by-controls

lists the zones for which no scoped sizing controls have been defined.

modify

modifies the scoped size control definition.

read

enables you to read in a scoped sizing file (*.szcontrol).

validate

validates the scoped sizing controls defined. An error will be reported if the scoped sizing controls do not

exist or the scope for one (or more) controls is invalid.

write

validate

write

enables you to write a scoped sizing file (*.szcontrol).

Chapter : size-functions/

Size functions can be defined using the commands in the size-functions menu. The command

size-functions/create enables you to define size functions. You need to specify the size function

type, whether face or edge zones are to be used, the boundary or edge zones for which the size function

is to be defined, the size function name, and the parameters relevant to the size function type. You can

also have the name generated automatically by retaining the default entry for the size function name.

The size function name will be assigned based on the zone type (face or edge) and the size function

type (for example, the size function face-curvature-sf- indicates that the curvature size function is

defined for face zones. The size function ID is .)

An example is

size-functions/create curvature face wall:x wall:y, curv-size-function . . .

where, curvature is the size function type, face indicates that face zones are to be used, wall:x,

wall:y indicate the boundary zones for which the size function is defined, and curv-size-function

is the size function name. The remaining values correspond to the parameters for the curvature size

function, that is, minimum and maximum size, growth rate, and normal angle.

Note

All boundary face zones and edge zones included in the global domain are available for

defining size functions, even if a local domain has been activated.

compute

computes the size function based on the defined parameters.

contours/

contains options for managing contours.

draw

compute

contours/

draw

displays contours in the graphics window. Run compute prior to contours/draw.

set/

contains options to manage the contour size.

refine-facets?

allows you to specify smaller facets if the original are too large. Default is no.

create

delete

enable-periodicity-filter

applies periodicity to the size field.

Specify the angle, pivot, and axis of rotation to set up periodicity.

If periodicity has been previously defined, the existing settings will be applied.

Note

Only rotational periodicity is supported, translational periodicity is not supported currently.

list

Note

If you set the global minimum size to a value greater than the local minimum size defined

for existing proximity, curvature, or hard size functions, a warning will appear, indicating

that the global minimum size cannot be greater than the specified local minimum size.

sets the tolerance relative to minimum size to take gaps into account. Gaps whose thickness is less than

the global minimum size multiplied by this factor will not be regarded as a proximity gap.

allows you specify the scale factor, and minimum and maximum size values to filter the size output from

identifies the zones comprising non-triangular elements and uses a triangulated copy of these zones for

computing the size functions.

allows you to disable curvature data from the nodes of the CAD facets.

Chapter : switch-to-solution-mode

switch-to-solution-mode

enables you to transfer the mesh data from meshing mode to solution mode in ANSYS Fluent.When you

use the switch-to-solution-mode command, you will be asked to confirm that you want to switch

to solution mode.

Appendix A. Query and Utility Functions

The following sections describe the query and utility functions available:

A.. List Queries and Utility Functions

A.. Label Utility Functions

A.. Report Utility Functions

A.. Diagnostic Based Marking Utility Functions

A.. Mesh Setup Utility Functions

A.. Mesh Operation Utility Functions

A.. Miscellaneous Functions

When performing a series of operations, you may want to list all the zones of a particular type, group,

or containing a particular text string or name pattern. You can also query zones through the TUI based

on a regular expression and a specified variable. You can:

Identify face/cell zones closest to a specified location.

Identify zones/objects of a specific type or containing a particular text string.You can also identify zones

belonging to a group or object.

Obtain object region and face zone label lists.

Obtain mesh setup information such as zones with prism mesh settings or prism controls defined

Use the utility functions to determine the zones created during a particular operation by performing Boolean

operations on lists returned by specific functions.

Use the eval-expr function to evaluate the lists returned by the functions in order that they can be used

as input in the text user interface commands.

Note

These functions are not supported in a distributed parallel environment.

Utility Function

Feature

(get-face-zone-at-location

'(x y z))

Return face zone at or closest to a

specified location.

Note

This function is not

applicable to

polyhedra meshes.

By location

Zone

query

Feature

(get-cell-zone-at-location

'(x y z))

Return cell zone at or closest to a

specified location

(get-zones-of-type 'type)

Return a list of zones of the specified

default zone type

By zone

type

Zone lists

(get-zones-of-group 'group)

default zone group or user-defined

group

By default

group

(get-face-zones-of-filter

'filter)

Return a list of zones whose names

contain the specified filter string

By filter

string

(get-cell-zones-of-filter

'filter)

(get-edge-zones-of-filter

'filter)

(get-node-zones-of-filter

'filter)

(get-face-zones-of-objects

'(object-list))

Return a list of face zones in the

specified objects

By object

(tgapi-util-get-face-zone-

id-list-of-object 'object)

Return a list of face zones by ID in the

specified object

By object

id-list-of-object "object")

id-list-of-regions 'object

'(region-list))

specified regions of an object

id-list-of-regions "object"

(get-edge-zones-of-objects

Return a list of edge zones in the

(tgapi-util-get-edge-zone-

Return a list of edge zones by ID in

the specified object

(tgapi-util-get-cell-zone-

Return a list of cell zones by ID in the

(get-face-zones-of-labels

'object '(list-of-label-

names))

specified face zone labels of the

object specified

id-list-of-labels 'object

'(face-zone-label-list))

specified face zone labels of an object

Query and Utility Functions

Feature

id-list-of-labels "object"

(get-face-zones-shared-by-

regions-of-type 'mesh-ob-

ject 'region-type)

Return a list of face zones shared by

regions of specified types in the mesh

object specified, where region-

type is fluid-fluid, solid-

solid, or fluid-solid

(get-face-zones-of-regions

'object '(list-of-region-

names))

specified regions

(tgapi-util-get-prism-cell-

zones '(zone-list))

Return a list of prism cell zones

By cell

shape

names))

By cell

shape

zones "zone-name-pattern*")

(tgapi-util-get-tet-cell-

Return a list of tet cell zones

(tgapi-util-get-adjacent-

cell-zones zone-id)

Return adjacent cell zones for given

face zone

By

connectivity

cell-zones 'zone-name)

cell-zones "zone-name")

face-zones '(cell-zone-

list))

Return adjacent boundary face zones

for given cell zones.

face-zones "cell-zone-name-

pattern*")

interior-and-boundary-face-

zones '(cell-zone-list))

Return adjacent interior and boundary

face zones for given cell zones.

zones "cell-zone-name-pat-

tern*")

zones-by-edge-connectivity

'(zone-list))

Return adjacent zones based on edge

"zone-name-pattern*")

List Queries and Utility Functions

Feature

zones-by-node-connectivity

Return adjacent zones based on node

(tgapi-util-get-shared-

boundary-zones 'cell-zone-

name)

Returns the number of faces and the

boundary face zones that are shared

with the specified cell zones.

boundary-zones '(cell-zone-

list))

boundary-zones "cell-zone-

list))

name-pattern*")

(tgapi-util-get-interior-

zones-connected-to-cell-

Returns interior face zones connected

to given cell zones.

tern*")

(tgapi-util-get-face-zones-

with-zone-specific-prisms-

applied)

Return a list of face zones with

zone-specific prism settings applied

Mesh setup

of-prism-controls "control-

name")

Return a list of face zones to which

the specified prism controls apply

(tgapi-util-get-baffles

'(face-zone-list))

Return the baffle zones based on the

face zone list specified

(tgapi-util-get-embedded-

baffles)

Return the embedded baffle zones

(get-wrapped-zones)

Return a list of wrapped face zones

Wrapped

zones

(get-unreferenced-edge-

zones)

Unreferenced Return a list of unreferenced zones

zones

(get-unreferenced-face-

zones)

(get-unreferenced-cell-

zones)

zones-of-filter 'filter)

Return a list of unreferenced zones

whose names contain the specified

filter string

Feature

(tgapi-util-get-unrefer-

enced-face-zone-id-list-of-

pattern "pattern*")

by ID, whose names contain the

specified pattern

enced-cell-zone-id-list-of-

enced-edge-zone-id-list-of-

(tgapi-util-get-maxsize-

cell-zone-by-volume "pat-

tern*")

Return cell zone with maximum

volume for given list or pattern of cell

zones

Mesh

cell-zone-by-volume '(zone-

list))

cell-zone-by-count "pat-

tern*")

Return cell zone with maximum count

of elements for given list or pattern

of cell zones

cell-zone-by-count '(zone-

list))

(tgapi-util-get-minsize-

face-zone-by-area "pat-

tern*")

Return face zone with minimum area

for given list or pattern of face zones

face-zone-by-area '(zone-

list))

face-zone-by-count "pat-

tern*")

Return face zone with minimum count

of face zones

face-zone-by-count '(zone-

list))

list-by-maximum-entity-

Return a list of face zones with a

count below the maximum entity

count (maximum-entity-count)

count maximum-entity-count

only-boundary?)

specified. You can choose to restrict

the report to only boundary face

zones, if required (only-boundary?

set to #t or #f).

Return a list of edge zones with a

Feature

the report to only boundary edge

Feature

count maximum-entity-count)

Return a list of cell zones with a count

below the maximum entity count

(maximum-entity-count)

list-by-maximum-zone-area

maximum-zone-area)

maximum zone area below the max-

imum-zone-area specified.

list-by-minimum-zone-area

minimum-zone-area)

minimum zone area above the min-

(tgapi-util-get-zones-with-

free-faces '(zone-id-list))

Return a list of zones with free faces

for the face zones specified

Mesh

diagnostics

free-faces '(zone-name-

list))

free-faces "zone-name-pat-

tern*")

multi-faces '(zone-id-

list))

Return a list of zones with

multi-connected faces for the face

zones specified

multi-faces '(zone-name-

list))

multi-faces "zone-name-pat-

tern*")

(tgapi-util-get-overlap-

ping-face-zones "face-zone-

Return a list of overlapping face zones

based on the area-tolerance and

distance-tolerance specified

name-pattern*" area-toler-

ance distance-tolerance)

marked-faces '(zone-id-

list))

Return a list of zones with marked

faces for the face zones specified

marked-faces '(zone-name-

list))

marked-faces "zone-name-

(tgapi-util-get-all-object-

name-list)

Return a list of all objects

By name

Object

lists

list))

By name

Object

lists

Feature

Return a list of objects of the specified (get-objects-of-type 'type)

type

By type

(tgapi-util-get-object-

name-list-of-type 'type)

(get-objects-of-filter

'filter)

Return a list of objects whose names

By filter

(get-regions-of-object 'ob-

ject)

Return a list of regions in the

By object

Region

lists

(tgapi-util-get-region-

name-list-of-object 'ob-

ject)

name-list-of-object "ob-

ject")

(get-regions-of-filter 'ob-

ject 'filter)

specified object, whose names

By filter

name-list-of-pattern 'ob-

contain the specified name pattern

By name

pattern

ject "region-name-pat-

tern*")

name-list-of-pattern "ob-

ject" "region-name-pat-

tern*")

(get-regions-of-face-zones

'(list-of-face-zone-IDs))

Return a list of regions containing the

face zones specified

By face

zones

name-list-of-face-zones

"face-zone-name-pattern*")

(tgapi-util-find-join-pairs

'(face-zone-name-list)

Return the pairs of overlapping face

zones based on the join tolerance and

Based on

join

tolerance

and feature

angle

Overlapping

zone pairs

join-tolerance absolute-

tolerance? join-angle)

Specify the face zones using a

Based on

join

tolerance

angle

zone pairs

face-zone-name-list, face-

'(face-zone-id-list) join-

zone-ID-list, or face-zone-

name-pattern*.

tolerance absolute-toler-

ance? join-angle)

"face-zone-name-pattern*"

Specify the tolerance value for

locating the overlapping faces

(join-tolerance).

Choose to use an absolute tolerance

value or relative to face edges (set

Feature

absolute-tolerance to #t or

#f).

Specify the feature angle to identify

features in the overlap region

(feature-angle).The default

value is .

Each member in the list returned

includes the zone IDs for the

overlapping zone pair and the

join region represented by the

bounding box. The same pair of

zones may appear multiple times

(with different join region

bounding box coordinates) in the

returned list.

The returned list is of the format:

((pair1_zone-id1

pair1_zone-id2 (join-re-

gion-bounding-box-min x y

z) (join-region-bounding-

box-max x y z))

(pair2_zone-id1 pair2_zone-

id2 (join-region-bounding-

box-min x y z) (join-re-

gion-bounding-box-max x y

z)) ...)

For example:

((  (-. -. -

.) (. -. -

.)) (  (-. -

. -.) (. -

. -.)) (  (-

. . -.)

(. . -.)))

(tgapi-util-convert-zone-

name-symbols-to-ids '(zone-

name-list))

Convert a list of zone name symbols

to a list of IDs

Convert

List

operations

name-strings-to-ids '(zone-

Convert a list of zone name strings to

a list IDs

Convert

List

a list IDs

ids-to-name-strings '(zone-

id-list))

Convert a list of zone IDs to a list of

name strings

ids-to-name-symbols '(zone-

id-list))

name symbols

Feature

(tgapi-util-convert-symbol-

list-to-string '(symbol-

list))

Convert a list of symbols to strings

(tgapi-util-create-string-

from-symbol-list '(symbol-

list))

Create a string from a list of symbols

(tgapi-util-integer-list-

subtract '(list-) '(list-

))

Returns the boolean subtraction of

the lists

Subtract

(tgapi-util-list-replace

new-element old-element

input-list)

Enables you to replace one element

in a list by another

Replace

(tgapi-util-remove-element-

from-list input-list ele-

ment)

Enables you to remove an element

from a list

Remove

(tgapi-util-list-contains?

input-list element)

Enables you to search for an element

in a list.

Search

A... Using Boolean Operations with Lists

You can perform Boolean operations on lists returned by the query functions:

Union of lists: (list-union list- list- ...)

Intersection of lists: (list-intersection list- list- ...)

Subtraction of lists: (list-subtract list- list-)

Note

Only two lists can be used as arguments for the subtraction operation.

list- = '(   )

list- = '(  )

list- = '(  )

then:

(list-union list- list- list-) = '(      )

(list-intersection list- list- list-) = '()

(list-subtract list- list-) = '(  )

A... Examples

Smoothing the prism-cap zone created during the prism creation operation:

– Obtain a list of the zones named prism-cap*.

(define initial-zones(get-face-zones-of-filter 'prism-cap*))

– Apply appropriate prism parameters and create prisms.

– Obtain a list of the zones named prism-cap* after the prism creation operation.

(define final-zones(get-face-zones-of-filter 'prism-cap*))

– Smooth the recently created prism-cap zone.

/boundary/improve/smooth(eval-expr '(list-subtract final-zones initial-

zones))

Improving mesh object quality:

/objects/improve-object-quality (get-objects-of-type 'mesh) smooth-and-

improve  no

Recovering periodic surfaces for mesh object face zones:

/boundary/recover-periodic-surfaces auto (get-face-zones-of-label

'_fluid '(periodic-))

Defining curvature sizing for all object face zones except symmetry planes:

/scoped-sizing/create control-curv curvature object-faces yes no "(eval-

expr ’(list-subtract (get-objects-of-filter '*) (get-objects-of-filter

'sym*)))" . .

The following label utility functions are available:

Function

Feature

(tgapi-util-add-labels-on-face-

zones '(face-zone-name-list)

'(label-name-list))

Add labels on the specified face zones.

On

face

zones

Add

labels

Specify the face zones using a face-

zone-name-list, face-zone-ID-

zones '(face-zone-ID-list)

list, or face-zone-name-pat-

tern*.

zones "face-zone-name-pattern*"

Specify the labels using a label-name-

list (for example '(label1 la-

bel2)).

tern*.

bel2)).

(tgapi-util-add-labels-on-cell-

zones '(cell-zone-name-list)

Add labels on the specified cell zones.

On

cell

zones

Specify the cell zones using a cell-

zone-name-list, cell-zone-ID-

zones '(cell-zone-ID-list)

list, or cell-zone-name-pat-

tern*.

Function

Feature

zones "cell-zone-name-pattern*"

bel2)).

(tgapi-util-add-labels-on-edge-

zones '(edge-zone-name-list)

Add labels on the specified edge zones.

On

edge

zones

Specify the edge zones using an edge-

zone-name-list, edge-zone-ID-

zones '(edge-zone-ID-list)

list, or edge-zone-name-pat-

tern*.

zones "edge-zone-name-pattern*"

bel2)).

(tgapi-util-get-labels-on-face-

zones '(face-zone-name-list))

Returns the list of labels for the specified

face zones. Specify the face zones using a

face-zone-name-list, face-zone-

On

face

zones

Return

list of

labels

zones '(face-zone-ID-list))

ID-list, or face-zone-name-pat-

tern*.

zones "face-zone-name-pat-

tern*")

(tgapi-util-get-labels-on-cell-

zones '(cell-zone-name-list))

cell zones. Specify the cell zones using a

tern*")

cell-zone-name-list, cell-zone-

On

cell

zone

zones '(cell-zone-ID-list))

ID-list, or cell-zone-name-pat-

tern*.

tern*")

(tgapi-util-get-labels-on-edge-

zones '(edge-zone-name-list))

edge zones. Specify the edge zones using

an edge-zone-name-list, edge-

On

edge

zone

zones '(edge-zone-ID-list))

zone-ID-list, or edge-zone-name-

pattern*.

zones "edge-zone-name-pat-

tern*")

(get-labels-of-object 'object)

Return a list of face zone labels in the

specified object.

Face

Zone

(get-labels-of-object "object")

Label

(tgapi-util-get-all-label-name-

list 'object)

lists

by

object

list "object")

(get-labels-of-filter 'object

'filter)

specified object, whose names contain the

specified filter/pattern string.

Label Utility Functions

Function

Feature

(tgapi-util-get-label-name-

list-of-pattern 'object "label-

list-of-pattern "object" "la-

bel-name-pattern*")

(get-labels-of-face-zones

Return a list of face zone labels containing

the face zones specified.

Face

Zone

Label

lists

by

face

zones

(tgapi-util-get-face-zone-id-

list-with-labels '(face-zone-

name-list) '(label-name-list))

Returns the list of face zones (by ID)

containing the labels specified.

Face

zones

Return

list of

Face

zones

Return

list of

zones

with

labels

tern*.

ID-list) '(label-name-list))

list-with-labels "face-zone-

bel2)).

name-pattern* '(label-name-

list))

(tgapi-util-get-cell-zone-id-

list-with-labels '(cell-zone-

Returns the list of cell zones (by ID)

Cell

Zones

tern*.

list-with-labels "cell-zone-

bel2)).

list))

(tgapi-util-get-edge-zone-id-

list-with-labels '(edge-zone-

Returns the list of edge zones (by ID)

Edge

zones

Specify the face zones using an edge-

tern*.

list-with-labels "edge-zone-

bel2)).

list))

Function

Feature

bel2)).

list))

Function

Feature

(tgapi-util-remove-labels-on-

face-zones '(face-zone-name-

list) '(label-name-list))

Removes the specified labels from the face

zones.

From

face

zones

Remove

labels

from

zones

face-zones '(face-zone-ID-list)

tern*.

face-zones "face-zone-name-pat-

tern*" '(label-name-list))

bel2)).

cell-zones '(cell-zone-name-

Removes the specified labels from the cell

zones.

From

cell

zones

cell-zones '(cell-zone-ID-list)

tern*.

cell-zones "cell-zone-name-pat-

bel2)).

edge-zones '(edge-zone-name-

Removes the specified labels from the edge

zones.

From

edge

zones

edge-zones '(edge-zone-ID-list)

tern*.

edge-zones "edge-zone-name-pat-

bel2)).

tern*.

bel2)).

Consider a model with face zones part1, part2, part3, inlet1, inlet2, and outlet.

(tgapi-util-add-labels-on-face-zones '(inlet1 inlet2) '(inlet))

(tgapi-util-add-labels-on-face-zones "part*" '(wall solid))

Return the list of labels on the specified face zone.

(tgapi-util-get-labels-on-face-zones '( ))

Returns list of labels: (inlet)

(tgapi-util-get-labels-on-face-zones "part*")

Returns list of labels: (wall solid)

Remove labels from the specified face zones.

(tgapi-util-remove-labels-on-face-zones "part*" '(solid))

Return the list of face zones (by ID) containing the labels specified.

(tgapi-util-get-face-zone-id-list-with-labels "inlet*" '(inlet))

Returns face zone ID list: ( )

The following functions are available for reporting mesh quality, statistics, face/cell distribution:

Feature

(tgapi-util-get-zone-type

zone-id)

Return zone type as integer

Report Mesh Types

zone-name)

shape zone-id)

Return cell zone shape as symbol

count '(zone-id-list))

Return count of entities for face zones

Report Mesh

count '(zone-name-list))

count "zone-name-pattern*")

Return count of entities for cell zones

node-count 'zone-id)

Returns the node count for the specified

face zone.

node-count 'zone-name)

node-count "zone-name")

area '(zone-id-list))

Return face zone area for the specified

zones

area '(zone-name-list))

Feature

area "zone-name-pattern*")

volume '(zone-id-list))

Return cell zone volume for the specified

zones

volume '(zone-name-list))

volume "zone-name-pattern*")

(tgapi-util-get-face-mesh-

distribution '(face-zone-

Report the face mesh distribution based

on the specified measure, parti-

tions, and range (such as (. )).

Specify the "measure" as one of

list) "measure" partitions

'(range))

distribution "face-zone-name-

pattern*" "measure" parti-

tions '(range))

"Skewness"

"Equiangle Skewness"

"Size Change"

"Edge Ratio"

"Size"

"Aspect Ratio"

"Squish"

"Warp"

"Dihedral Angle"

"ICEMCFD Quality"

"Ortho Skew"

"FLUENT Aspect Ratio"

"Inverse Orthogonal Qual-

ity"

(tgapi-util-get-cell-mesh-

distribution '(cell-zone-

Report the cell mesh distribution based

'(range))

distribution "cell-zone-name-

'(range))

Report Utility Functions

Feature

"Size"

"Squish"

"Warp"

ity"

(tgapi-util-get-face-quality-

limits '(face-zone-list)

"measure")

Report the worst quality face and face

quality limits (minimum, maximum,

average quality) for the list of zones

based on the measure specified. You

can also report face size limits.

Report Quality/Size

Limits

limits "face-zone-name-pat-

tern*" "measure")

"Size"

"Squish"

"Warp"

Feature

ity"

(tgapi-util-get-cell-quality-

limits '(cell-zone-list)

Report the number of cells and the cell

can also report the cell size limits.

limits "cell-zone-name-pat-

"Size"

"Squish"

"Warp"

ity"

(tgapi-util-print-worst-qual-

"Size"

"Squish"

"Warp"

ity"

ity-cell '(cell-zone-list)

Report the worst quality cell (ID and

location) for the cell zones based on the

measure specified.

ity-cell "cell-zone-name-pat-

Feature

"Size"

"Squish"

"Warp"

ity"

(tgapi-util-get-edge-size-

limits '(face-zone-list))

Report the edge size limits for the list of

face zones

tern*")

(tgapi-util-get-free-faces-

count '(face-zone-name-list))

Returns the count of free faces for the

Report count

count '(face-zone-id-list))

count "face-zone-name-pat-

tern*")

(tgapi-util-get-multi-faces-

Returns the count of multi-connected

tern*")

(tgapi-util-count-marked-

faces '(face-zone-name-list))

Returns the count of marked faces for

the face zones specified

faces '(face-zone-id-list))

faces "face-zone-name-pat-

tern*")

Feature

(tgapi-util-print-dia-

tern*")

Feature

gnostics-summary '(object-

Print the diagnostics summary for a list

of objects

Print summary

(tgapi-util-mesh-check "type-

name" '(edge-zone-list)

Reports the selected mesh check

statistics for the zones specified.

Mesh check

'(face-zone-list) '(cell-

zone-list))

Specify the "type-name" as one of

name" "edge-zone-name-pat-

– "bounding-box-statistics"

tern*" '(face-zone-list)

'(cell-zone-list))

– "volume-statistics"

– "face-area-statistics"

– "nodes-per-edge"

– "nodes-per-face"

– "nodes-per-cell"

tern*" "face-zone-name-pat-

tern*" '(cell-zone-list))

– "faces-or-neighbors-per-

cell"

'(face-zone-list) "cell-zone-

– "cell-faces-or-neighbors"

– "isolated-cells"

– "face-handedness"

tern*" "cell-zone-name-pat-

tern*")

– "periodic-face-pairs"

– "face-children"

– "zone-boundary-conditions"

– "invalid-node-coordinates"

– "poly-cells"

– "parallel-invalid-zones"

– "parallel-invalid-neighbor-

hood"

– "parallel-invalid-inter-

faces"

Refer to Checking the Mesh in the

Fluent User's Guide for

descriptions of the individual

mesh checks.

Feature

Specify the zones to be checked.

Specify the edge zones (edge-

Feature

zone-list or edge-zone-

name-pattern*), face zones

(face-zone-list or face-

zone-name-pattern*), and

cell zones (cell-zone-list or

cell-zone-name-pattern*).

The following functions are available for identifying faces/zones based on diagnostic criteria such as

face connectivity and quality:

Feature Description

(tgapi-util-mark-free-faces '(zone-

id-list))

Mark free faces on the face zones specified

(tgapi-util-mark-free-faces "zone-

(tgapi-util-mark-multi-faces '(zone-

id-list) n)

Mark multi-connected faces on the face zones

specified based on fringe length (n)

name-list) n)

(tgapi-util-mark-multi-faces "zone-

name-pattern*" n)

(tgapi-util-mark-self-intersecting-

faces '(zone-id-list) mark-folded?)

Mark self-intersecting faces on the face zones

specified. Specify whether to mark folded faces or

not (mark-folded? set to #t or #f).

faces '(zone-name-list) mark-folded?)

faces "zone-name-pattern*" mark-fol-

ded?)

(tgapi-util-mark-faces-in-self-prox-

imity '(zone-id-list) relative-toler-

Mark faces in self-proximity on the face zones

specified. Specify whether to use relative tolerance

(relative-tolerance? set to #t or #f), tol-

ance? tolerance angle ignore-orient-

ation?)

erance value, the angle, and whether to ignore

orientation (ignore-orientation? set to #t

or #f).

ation?)

or #f).

imity '(zone-name-list) relative-

tolerance? tolerance angle ignore-

orientation?)

imity "zone-name-pattern*" relative-

(tgapi-util-mark-duplicate-faces

'(zone-id-list))

Mark duplicate faces on the face zones specified

'(zone-name-list))

(tgapi-util-mark-invalid-normals

Mark invalid normal locations on the face zones

specified

(tgapi-util-mark-point-contacts

Mark point contact locations on the face zones

specified

(tgapi-util-mark-island-faces '(zone-

Mark island faces on the face zones specified, based

on the island face count (n)

(tgapi-util-mark-island-faces "zone-

(tgapi-util-mark-spikes '(zone-id-

list) spike-angle)

Mark spikes on the face zones specified, based on

the spike angle (spike-angle)

(tgapi-util-mark-spikes '(zone-name-

(tgapi-util-mark-spikes "zone-name-

pattern*" spike-angle)

(tgapi-util-mark-steps '(zone-id-

list) step-angle step-width)

Mark steps on the face zones specified, based on

the step angle (step-angle) and step width

(step-width)

(tgapi-util-mark-steps '(zone-name-

(tgapi-util-mark-steps "zone-name-

pattern*" step-angle step-width)

(tgapi-util-mark-sliver-faces '(zone-

id-list) max-height skew-limit)

Mark sliver faces on the face zones specified, based

on the maximum height (max-height) and

skewness limit (skew-limit)

name-list) max-height skew-limit)

Diagnostic Based Marking Utility Functions

(tgapi-util-mark-sliver-faces "zone-

name-pattern*" max-height skew-limit)

(tgapi-util-mark-bad-quality-faces

'(zone-id-list) quality-limit nrings)

Mark bad quality faces on the boundary face zones

specified, based on the quality limit (quality-

limit) and number of rings (nrings).

'(zone-name-list) quality-limit

nrings)

"zone-name-pattern*" quality-limit

nrings)

(tgapi-util-mark-faces-by-quality

'(zone-id-list) quality-measure

quality-limit append-marking?)

Mark faces based on the quality-measure and

quality-limit specified. Specify whether to

append the faces to those previously marked or

clear previously marked faces (append-marking?

set to #t or #f)

'(zone-name-list) quality-measure

"zone-name-pattern*" quality-measure

(tgapi-util-mark-face-strips-by-

height-and-quality '(zone-id-list)

Mark face strips based on the strip-type,

strip-height, quality-measure, quality-

strip-type strip-height quality-

measure quality-limit feature-angle)

limit, and feature-angle specified. Possible

values for strip-type are:

height-and-quality '(zone-name-list)

: boundary-boundary strip. Multi-connected face

edges are also considered as boundary here.

: feature-feature strip between angle based

features. Feature edges, multi-connected edges,

and free edges are angle based features. Boundary height-and-quality "zone-name-pat-

edges will be considered features if there is an

angle.

tern*" strip-type strip-height qual-

ity-measure quality-limit feature-

angle)

: all-all strip between all boundaries and features.

: pure feature-feature strip. Only pure features,

boundary edges and multi edges will not be

considered as pure feature edges even if there is

an angle based feature.

The recommended value is .

(tgapi-util-mark-faces-deviating-

from-size-field '(zone-id-list) min-

Mark all faces at nodes based on deviation from

size-factor max-size-factor "sf-type-

to-compare")

Specify the zones using zone-id-list, zone-

name-list, or zone-name-pattern*.

Specify the min-size-factor and max-size- from-size-field '(zone-name-list)

factor.

min-size-factor max-size-factor "sf-

type-to-compare")

Specify the size field type to be used to get size

at node. Set "sf-type-to-compare" to

"volumetric" or "geodesic".

from-size-field "zone-name-pattern*"

Faces will be marked if the minimum edge length

at the node is less than min-size-

factor×size-at-node or the maximum edge

length is greater than max-size-factor×size-

at-node.

(tgapi-util-mark-faces-using-node-

degree '(zone-id-list) node-degree-

threshold)

Mark all faces with node degree above the specified

threshold. Node degree is defined as the number

of edges connected to the node.

degree '(zone-name-list) node-degree-

Specify the face zones using zone-id-list,

zone-name-list, or zone-name-pattern*.

degree "zone-name-pattern*" node-de-

gree-threshold)

Specify the node-degree-threshold.

The following functions are available for mesh setup:

(get-average-bounding-box-center

'(face-zone-ID-list))

Return a suitable average point based on the zones

specified

(tgapi-util-get-bounding-box-of-zone-

list '(zone-id-list))

Return the bounding box extents for the list of

zones.

(tgapi-util-un-preserve-cell-zones

Enables you to unpreserve some/all preserved cell

zones during the meshing process.

"cell-zone-name-pattern*")

(tgapi-util-create-boi-and-size-

functions-from-refinement-regions

Create bodies of influence and if required body of

influence size functions from the mesh refinement

regions. Specify the refinement region type (set

"region-type" "boi-prefix-string"

create-size-function?)

"region-type" to "tet" or "hexcore").

Specify the prefix for the BOI zones ("boi-pre-

fix-string"), and choose whether to create the

size functions (set create-size-function? to

#t or #f).

(tgapi-util-scale-face-zones-around-

pivot '(face-zone-list) '(scale)

'(pivot) use-bbox-center?)

Enables you to scale the face zones around a pivot

point or the bounding box center. Specify the face

zones, the scale factors in the X, Y, Z directions

(scale), the pivot point (pivot), and choose

pivot "face-zone-name-pattern*"

'(scale) '(pivot) use-bbox-center?)

whether to use the bounding box center (use-

bbox-center? set to #t or #f).

Mesh Setup Utility Functions

(tgapi-util-scale-cell-zones-around-

pivot '(cell-zone-list) '(scale)

Enables you to scale the cell zones around a pivot

point or the bounding box center. Specify the cell

pivot "cell-zone-name-pattern*"

(tgapi-util-dump-face-zone-orienta-

tion-in-region "filename")

Return the face zones and their orientation for the

mesh file specified

(tgapi-util-sort-regions-by-volume

"object-name" "order")

Returns a sorted list of volumetric regions by

volume for the object specified. Specify the order

(ascending or descending).

(tgapi-util-get-region-volume 'ob-

ject-name 'region-name)

Return the region volume for the specified region

of an object

(tgapi-util-get-region-volume "ob-

ject-name" "region-name")

(tgapi-util-set-quality-measure

Set the quality measure.

Specify the "measure" as one of the

"Size"

"Squish"

"Warp"

"Inverse Orthogonal Quality"

(tgapi-util-set-object-cell-zone-type

'object 'cell-zone-type)

Set object cell zone type

"object" 'cell-zone-type)

(tgapi-util-set-number-of-parallel-

compute-threads nthreads)

Set the number of compute threads to use for

algorithms like mesh check and quality

computation. You can use a variable number of

compute threads for these algorithms depending

on the current machine loads. The number of

compute threads is between  and the value

(maximum-cores-available - ).

Feature

(tgapi-util-rename-face-zone

"zone-name" "new-name")

Renames an existing face zone

Rename zones

'zone-id "new-name")

(tgapi-util-rename-edge-zone

Renames an existing edge zone

(tgapi-util-replace-face-

zone-suffix '(face-zone-list)

Replace the face zone suffix to rename

face zones. Specify whether to merge

the face zones being renamed (set

merge? to #t or #f).

Note

If an empty string is

specified for the separ-

"separator" "replace-with"

merge?)

ator (" "), the string

specified for replace-

with will be appended

to the face zone names.

(tgapi-util-replace-cell-

zone-suffix '(cell-zone-list)

Replace the cell zone suffix to rename

cell zones. Specify whether to merge the

cell zones being renamed (set merge?

to #t or #f)

"old-suffix" "new-suffix"

merge?)

(tgapi-util-replace-edge-

zone-suffix '(edge-zone-list)

Replace the edge zone suffix to rename

edge zones. Specify whether to merge

the edge zones being renamed (set

merge? to #t or #f)

merge?)

(tgapi-util-remove-id-suffix-

from-face-zones)

Removes the ID suffix from face zone

names

(tgapi-util-clean-face-zone-

names)

Clean up face zone names by removing

IDs wherever possible

Mesh Operation Utility Functions

Feature

(tgapi-util-remove-ids-from-

zone-names '(zone-id-list))

Remove the zone ID (:id) from zone ID

list.

(tgapi-util-renumber-zone-ids

'(zone-id-list) start-number)

Renumber zone IDs starting from the

number specified (start-number).

Change zone ID

(tgapi-util-rename-object

"old-object-name" "new-ob-

ject-name")

Renames the object

Rename objects

(tgapi-util-replace-object-

suffix '(object-name) "separ-

ator" "new-suffix")

Rename objects by replacing the object

suffix with a new suffix

(tgapi-util-rename-label "ob-

ject-name" "old-label-name"

"new-label-name")

Renames the face zone label

Rename labels

(tgapi-util-replace-label-

suffix '(object-list) "separ-

Rename labels by replacing the label

(tgapi-util-copy-labels from-

face-zone to-face-zone)

Copy labels from one face zone to

another. Specify either face zone names

or IDs

Copy labels

(tgapi-util-merge-face-zones

Merges the specified face zones. Specify

a list of zone IDs or name pattern.

Merge zones

(tgapi-util-merge-face-zone-

of-type 'zone-type "zone-

Merges face zones of a given type based

on name pattern

(tgapi-util-merge-face-zones-

with-same-prefix "prefix")

Merges face zones containing the

specified prefix

(tgapi-util-merge-cell-zones

Merges the specified cell zones. Specify

a list of cell zones or name pattern.

(tgapi-util-merge-cell-zones-

Merge cell zones containing the specified

prefix

with-same-suffix "suffix")

suffix

(tgapi-util-separate-cell-

zone-layers-by-face-zone

Separates cells that are connected to

specified face zones into another cell

zone. This separation method applies

Separate

'(cell-zone-id) '(face-zone-

list) nlayers)

only to prism cells. Specify the number

of layers of cells (nlayers) to be

separated.

Separate

'(cell-zone-id) "face-zone-

name-pattern*" nlayers)

Feature

"cell-zone-name" '(face-zone-

"cell-zone-name" "face-zone-

(tgapi-util-separate-face-

zones-by-cell-neighbor

Separate face zones based on the cell

neighbors.

zones-by-cell-neighbor "face-

zone-name-pattern*")

(tgapi-util-refine-marked-

faces-in-zones '(face-zone-

list))

Refine marked faces

Refine

faces-in-zones "face-zone-

(tgapi-util-fill-holes-in-

face-zone-list '(face-zone-

list) max-hole-edges)

Fill holes associated with free edges for

the face zones specified, based on the

number of free edges (max-hole-

edges)

Patch

face-zone-list "face-zone-

name-pattern*" max-hole-

edges)

(tgapi-util-project-zone-on-

plane zone-id plane)

Project a zone on the plane specified.

Specify three points for defining the

plane.

Project

(tgapi-util-delete-all-sub-

domains)

Deletes all sub-domains (all domains

other than global)

Delete

(tgapi-util-delete-marked-

list))

Delete marked faces

(tgapi-util-delete-empty-

face-zones '(face-zone-list))

Delete empty zones based on the zones

specified

face-zones "face-zone-name-

specified

edge-zones '(edge-zone-list))

Feature

edge-zones "edge-zone-name-

cell-zones '(cell-zone-list))

cell-zones "cell-zone-name-

(tgapi-util-boundary-zone-ex-

ists? zone-id)

Report if the boundary face zone exists

Validate mesh

ists? 'zone-name)

(tgapi-util-interior-zone-ex-

Report if the interior face zone exists

(tgapi-util-cell-zone-exists?

zone-id)

Report if the cell zone exists

'zone-name)

(tgapi-util-mesh-exists?)

Report if the volume mesh exists

Feature

(tgapi-util-string-contains?

"string1*" "string2*")

Check if the string contains another

string

String operations

(tgapi-util-string-split

"original-string" "split-

character")

Enables you to split a string by the

specified character.

(tgapi-util-string-split-

with-string "original-string"

"split-string")

specified string.

(tgapi-util-string-replace

"target-string" "old-sub-

string" "new-sub-string")

For example: (tgapi-util-

string-replace "tst-

Enables you to replace a part (old-

sub-string) of a target-string

by the specified string (new-sub-

string).

string).

Feature

string" "tst" "test") will

return "test-string".

(tgapi-util-get-mesher-work-

ing-directory)

Returns the path for the working

directory

Folder/directory

(tgapi-util-sync-directories

directory)

Sync the Cortex current working

directory with the Fluent current working

directory (directory)

(tgapi-util-find-file-with-

suffix "filename" "file-suf-

fix")

Finds the file in the working directory

based on the filename and file-

suffix specified.

File management

(tgapi-util-find-file-pat-

tern-with-suffix "filename"

"file-suffix")

(tgapi-util-get-last-read-

file-name)

Returns the last read file

file-suffix)

Returns the file suffix for the last read

file

Miscellaneous Functions

Appendix B. Boundary Functions

The following boundary functions are available.

Note

Function

Feature

(tgapi-boundary-split-marked-

faces '(face-zone-id-list)

longer-edge-split-ratio)

Improve marked faces by splitting the

longer edge.

Improve surface

mesh

zone-id-list, face-zone-name-

faces '(face-zone-name-list)

tern*.

Specify the longer-edge-split-

ratio (length ratio for the split

tern*" longer-edge-split-ra-

tio)

created by projecting the opposite

node onto the longer edge).The valid

tio)

range is  to . and the

recommended value is ..

(tgapi-boundary-collapse-

marked-faces '(face-zone-id-

Improve marked faces by collapsing face

edges.

list) preserve-boundary?

boundary-corner-angle max-

collapsible-edge-ratio)

tern*.

marked-faces '(face-zone-

name-list) preserve-boundary?

Choose whether to preserve the

boundary by setting preserve-

boundary? to #t or #f.

marked-faces "face-zone-name-

– If preserve-boundary? is

enabled (#t), specify the bound-

pattern*" preserve-boundary?

ary-corner-angle to be used

for marking fixed nodes on the

boundary.The recommended value

is  degrees.

Set the max-collapsible-edge-

ratio depending on the improve

operation:

Function

Feature

To improve general quality, specify

a value between  to .. A value

of . is recommended.

–

– To collapse sliver faces, specify a

value of ..

Note

A value of  will result

in all marked faces

being collapsed.

Tip

Use this operation when

the mesh skewness is

Also, it is recommended

to mark faces and

collapse faces by edge

ratio incrementally. For

example, first mark faces

with skewness greater

than . and then

collapse marked faces

using an edge ratio of

.. When the mesh

quality is improved, next

mark faces with

skewness greater than

. and then collapse

marked faces using an

edge ratio of . ; and so

on.

(tgapi-boundary-split-and-

collapse-sliver-faces '(face-

Improve sliver faces by splitting and

collapsing edges.

zone-id-list) sliver-height

"sliver-quality-measure"

sliver-quality longer-edge-

tern*.

split-ratio preserve-bound-

ary? boundary-corner-angle)

Specify the height threshold for sliver

face improvement. All faces with

zone-name-list) sliver-height

sliver-height less than the

specified value will be marked for

Boundary Functions

Function

Feature

improvement. Sliver height is the

shortest height of the triangular face -

the distance between the location of

the opposite node and its projection

point on the longer edge.

collapse-sliver-faces "face-

zone-name-pattern*" sliver-

Specify either "Skewness" or "As-

pect Ratio" as the "sliver-

height "sliver-quality-meas-

ure" sliver-quality longer-

quality-measure", and the

edge-split-ratio preserve-

sliver-quality threshold used for

marking.

boundary? boundary-corner-

angle)

(tgapi-boundary-fill-planar-

holes-using-free-faces

Create a planar surface to patch holes

associated with free faces for the face

zones specified. The free faces should be

Patch

'(face-zone-id-list) plane

continuous for the planar patch to be

created.

ance?)

Specify the face zones with free faces

using a face-zone-id-list,

'(face-zone-name-list) plane

face-zone-name-list, or face-

zone-name-pattern*.

ance?)

holes-using-free-faces "face-

Specify three coplanar points to define

the plane (for example, (list '(-

) '(  ) '( -

))).

zone-name-pattern*" plane

ance?)

Specify the tolerance value, and

choose whether to use an absolute

tolerance (set absolute-toler-

ance? to #t or #f). Nodes within the

Function

Feature

tolerance from the plane will be used

to create the planar surface.

Note

The patch surface is not

connected to the original

holes-using-free-faces-in-ob-

associated with free faces for the object

and face zone labels specified. The free

ject 'object '(face-zone-la-

faces should be continuous for the

planar patch to be created.

bel-list) plane tolerance

absolute-tolerance? "new-la-

bel-name")

Specify the object and the face zone

labels with free faces using a face-

zone-label-list or face-zone-

label-name-pattern*.

ject 'object "face-zone-la-

bel-name-pattern*" plane

tolerance absolute-tolerance?

) '(  ) '( -

))).

ject "object" '(face-zone-

label-list) plane tolerance

ject "object" "face-zone-la-

Specify the new-label-name for the

planar surface created.The patch

surface is included in the object and a

new face zone label is created.

(tgapi-boundary-create-

planar-surface-using-edges

using the free face edges for the edge

zones specified. The edge zone should

'(edge-zone-id-list) plane

be continuous and free from

intersections.

ance?)

Specify the edge zones using an

edge-zone-id-list, edge-zone- '(edge-zone-name-list) plane

name-list, or edge-zone-name-

pattern*.

ance?)

pattern*.

ance?)

Function

Feature

) '(  ) '( -

))).

"edge-zone-name-pattern*"

plane tolerance absolute-

tolerance?)

Note

(tgapi-boundary-remesh-

Remesh the marked faces.

Remesh

list) n-rings preserve-

shared-zone-boundary? fea-

tern*.

ture-min-angle feature-max-

angle corner-angle "sizing-

option" constant-size min-

size max-size growth-rate)

Specify the number of rings (n-

rings).

Choose whether to preserve the shared marked-faces '(face-zone-

zone boundary by setting preserve- name-list) n-rings preserve-

shared-zone-boundary? to #t or

#f (recommended).

Specify the feature-min-angle

and feature-max-angle.The

feature-min-angle and fea-

ture-max-angle are the limits for

the feature angle. Recommended

pattern*" n-rings preserve-

values are  and , respectively. If

the mesh has false features like folds

and overlaps, the feature-max-

angle can be set to .

Specify the corner-angle.The

corner-angle is the minimum angle

between feature edges that will be

preserved during remeshing.The

recommended value is .

Select a "sizing-option" using

"geometric", "constant",

"geodesic" or "volumetric".

Function

Feature

Specify values for constant-size

(used when "sizing-option" is set

to "constant"), min-size, max-

size, and growth-rate (these are

used when "sizing-option" is set

to "geometric" or "geodesic").

Note

All four values must

be provided regardless

of the selected "siz-

ing-option".

A value of - can be

used for the

parameters that are

not required for a

particular sizing

option.

(tgapi-boundary-remesh-face-

zones '(face-zone-list)

Remesh face zones by separating them

internally into patches and later merging

them. The patches which fail to remesh

'(edge-zone-list) replace-

using the advancing front (surfer)

face-zones? feature-min-angle

algorithm will be remeshed using explicit feature-max-angle corner-

remeshing (split, improve, and coarsen).

angle "sizing-option" con-

You can specify the number of attempts

stant-size min-size max-size

for the advancing front algorithm and

growth-rate n-retries-on-

also use explicit remeshing for the

patches, if required.

failed improve-failed? front-

intersection-tolerance)

Specify the face zones and edge zones

using a face/edge zone list or by

face/edge zone name pattern.

"edge-zone-name-pattern*" re-

place-face-zones? feature-

min-angle feature-max-angle

Choose whether to replace the original

zones with the remeshed zones by

corner-angle "sizing-option"

constant-size min-size max-

setting replace-face-zones? to

#t or #f (recommended).

size growth-rate n-retries-

on-failed improve-failed?

front-intersection-tolerance)

ture-max-angle limits are used to

tern*" '(edge-zone-list) re-

retain angle-based features.

Recommended values are  and ,

respectively. If the mesh has false

features like folds and overlaps, the

Function

Feature

feature-max-angle can be set to

.

corner-angle is the minimum angle (tgapi-boundary-remesh-face-

tern*" "edge-zone-name-pat-

preserved for corner nodes during

tern*" replace-face-zones?

remeshing.The recommended value

is .

feature-min-angle feature-

max-angle corner-angle "siz-

ing-option" constant-size

"constant", "geodesic" or

"volumetric".

Note

The "geometric"

option is not

min-size max-size growth-rate

n-retries-on-failed improve-

Note

failed? front-intersection-

tolerance)

to "geodesic").These values are not

used when the "sizing-option"

is set to "volumetric".

Note

option.

Specify the number of attempts to

improve the failed patches using

explicit remeshing (n-retries-on-

failed) and whether to further

Function

Feature

explicit remeshing improve-

failed? set to #t or #f.

Specify the front-intersection-

tolerance for checking intersections.

The value specified should be in the

range  to .The recommended value

is ., which can be increased if the

remeshed patch shows intersections.

(tgapi-boundary-remesh-ob-

ject-labels 'object-name

Remesh object face zone labels by

separating them internally into patches

and later merging them. The patches

'(face-zone-label-list)

which fail to remesh using the surfer

'(edge-zone-list) feature-

(advancing front) algorithm, will be

remeshed using explicit remeshing (split, corner-angle "sizing-option"

improve, and coarsen). You can specify

the number of attempts for the surfer

algorithm and also use explicit

remeshing for the patches, if required.

Specify the object, face zone labels

(face-zone-label-list or face-

zone-label-pattern*), and edge

zones (edge-zone-list or edge-

zone-name-pattern*).

"face-zone-label-pattern*"

.

corner-angle is the minimum angle constant-size min-size max-

is .

ject-labels "object-name"

Function

Feature

Note

Note

Note

option.

B.. Examples

To improve mesh quality on all face zones, use marking utilities with functions for improving the surface

mesh and remeshing.

Mark faces based on quality:

(tgapi-util-mark-faces-by-quality "*" "Skewness" . #f)

Improve the marked faces by splitting the longer edge.

(tgapi-boundary-split-marked-faces "*" .)

Improve sliver faces

(tgapi-boundary-split-and-collapse-sliver-faces "*" . "Skewness" .

. #t )

Mark face strips between all boundaries based on strip height and quality.

(tgapi-util-mark-face-strips-by-height-and-quality "*"  . "Skewness"

. )

Improve the marked faces by collapsing face edges.

(tgapi-boundary-collapse-marked-faces "*" #f  .)

Remesh the marked faces based on the size field:

(tgapi-boundary-remesh-marked-faces "*"  #f    "geodesic" .

. . .)

For a mesh object _fluid, remesh all face zones using different sizing options:

Using geodesic sizing

(tgapi-boundary-remesh-face-zones (tgapi-util-get-face-zone-id-list-of-

object "_fluid") (tgapi-util-get-edge-zone-id-list-of-object "_fluid")

#t    "geodesic" - . . #t .)

Using volumetric sizing

#t    "volumetric" - - - -  #t .)

Using constant sizing

#t    "constant" . - - -  #t .)

Note

In these examples, a value of - has been used for the parameters that are not required for

a particular sizing option.

For a mesh object _fluid, remesh object face zone labels using different sizing options:

(tgapi-boundary-remesh-object-labels "_fluid" "*" "*"

"geodesic" - . . #f .)

(tgapi-boundary-remesh-object-labels "_fluid" "*" "*"    "volu-

metric" - - - -  #f .)

(tgapi-boundary-remesh-object-labels "_fluid" "*" "*"    "con-

stant" . - - -  #f .)

Note

Patch holes associated with free faces.

Create a planar surface to patch holes associated with free faces for the list of face zones.

(tgapi-boundary-fill-planar-holes-using-free-faces '(   ) (list '(-

) '(  ) '( - )) . #t)

Create a planar surface to patch holes associated with free faces for the list of object face zone labels.

(tgapi-boundary-fill-planar-holes-using-free-faces-in-object "object"

"*" (list '(-  ) '(  ) '( - )) . "symmetry" #t)

Create a planar surface to patch holes using the free face edges for the edge zones specified.

(tgapi-boundary-create-planar-surface-using-edges "*" (list '(-  )

'(  ) '( - )) . #f)

Examples

Appendix C. Connect Functions

The following connect functions are available.

Note

Function

Examples

Note

Function

(tgapi-connect-join-across-label-

pairs 'object-name '(label-pairs)

Connect overlapping face zone label pairs by joining

zones across label pairs.

feature-angle tolerance absolute-

Specify the mesh object-name.

tolerance? separate-overlaps? "separ-

ate-method" remesh? "sizing-method"

no-of-layers)

Specify a list of face zone label-pairs to be

connected. For example, (label1 label2).

Specify values for the parameters:

– feature-angle (default is )

– tolerance (default is .)

– absolute-tolerance? Specify #t or #f

(default, for relative tolerance).

– separate-overlaps? Specify #t (default)

or #f to separate overlapping zones.

– "separate-method" Specify "keep-none"

or "keep-one" (recommended).

– remesh? Specify #t (default) or #f to remesh

after the connect operation.

– "sizing-method" Set to "geometric"

(default) or "size-field".

– no-of-layers Specify the number of rings

of faces to be remeshed around the

connections, default is .

(tgapi-connect-intersect-across-la-

bel-pairs 'object-name '(label-pairs)

Connect overlapping face zone label pairs by

intersecting zones across label pairs.

tolerance? separate-intersections?

remesh? "sizing-method" no-of-layers)

Function

– separate-intersections? Specify #t

(default) or #f to separate intersecting zones.

(tgapi-connect-stitch-across-label-

stitching zones across label pairs.

"stitch-method" feature-angle toler-

ance absolute-tolerance? remesh?

"sizing-method" no-of-layers)

– "stitch-method" Specify "all-all"

(default), "free-free", or "free-non-

free".

Connect Functions

Function

C.. Examples

For a mesh object _fluid with face zone labels part1, part2, and part3:

Connect overlapping face zone label pairs by joining zones across label pairs.

(tgapi-connect-join-across-label-pairs '_fluid (list '(part1 part2)

'(part1 part3) '(part2 part3))  . #f #t "keep-one" #t "geometric"

)

)

Connect overlapping face zone label pairs by intersecting zones across label pairs.

(tgapi-connect-intersect-across-label-pairs '_fluid (list '(part1 part2)

'(part1 part3) '(part2 part3))  . #f #t #t "geometric" )

Connect overlapping face zone label pairs by stitching zones across label pairs.

(tgapi-connect-stitch-across-label-pairs '_fluid (list '(part1 part2)

'(part1 part3) '(part2 part3)) "all-all"  . #f #t "geometric" )

Examples

Appendix D. Size Field Functions

The size field defines the sizes in the volume. Having volumetric sizes could pose problems where sizes

are diffused across dead space, leading to unnecessary refinement. In addition to volumetric sizing, a

new type of size definition (geodesic) is introduced to define the sizes along a surface rather than the

volume. The geodesic sizing enables you to confine sizes to surfaces and avoid problems like dead

space refinement.

The following size field functions are available.

Note

Function

Feature

(tgapi-size-field-initialize-

geodesic-on-face-zones

Initialize geodesic sizing on the specified

On face

zones

geodesic

sizing

'(face-zone-name-list) max-

size)

zone-id-list, face-zone-

name-list, or face-zone-name-

pattern*.

'(face-zone-ID-list) max-

size)

Specify the max-size value.

max-size)

geodesic-on-object-labels

size)

max-size)

object face zone labels.

On

object

face

'(object-list) '(face-zone-

label-list) max-size)

Specify the object-list or ob-

ject-name-pattern* and the face

zone

labels

zone labels using a face-zone-la-

bel-list or face-zone-label-

'(object-list) "face-zone-

label-name-pattern*" max-

size)

"object-name-pattern*"

'(face-zone-label-list) max-

size)

Function

Feature

"face-zone-label-name-pat-

tern*" max-size)

geodesic-on-objects '(ob-

ject-list) max-size)

Initialize geodesic sizing on the face

zones for the specified objects.

On

object

face

zones

ject-name-pattern*.

geodesic-on-objects "object-

name-pattern*" max-size)

(tgapi-size-field-compute-

geodesic '(size-control-

Computes geodesic sizes on face nodes

based on the size controls specified.

Geodesic

sizes

Compute

size

field

name-pattern*))

geodesic "size-control-name-

pattern*)

volumetric '(size-control-

Computes the volumetric size field

sizes

sizes

volumetric "size-control-

geodesic-blended '(size-con-

trol-name-list))

Computes the geodesic blended size

field as follows.

Geodesic

blended

size field

The volumetric size field is computed

based on all edge, face proximity and

BOI controls.

trol-name-pattern*))

geodesic-blended "size-con-

trol-name-pattern*")

Geodesic sizes are computed based

on the remaining size controls.

Updates geodesic sizes based on

volumetric sizes (the lower minimum

size (geodesic or volumetric) will be

used).

Hard sizes are computed last.

(tgapi-size-field-update-

geodesic-with-volumetric-on-

Updates nodal (geodesic) sizes based

on the existing volumetric size field for

the face zones specified. This requires

On face

zones

Update

geodesic

sizes

Size Field Functions

Function

Feature

with

volumetric

sizes

face-zones '(face-zone-id-

list))

the volumetric size field to be

computed.

face-zone-id-list, face-

list))

zone-name-list, or face-

Note

Geodesic sizes need to

be initialized and

computed before

attempting an update.

the face zone labels specified. This

On

object

face

object-labels 'object-name

zone

labels

requires the volumetric size field to be

computed.

Specify the object-name and the

face zone labels using a face-

'(face-zone-label-name-pat-

tern*))

zone-label-list or face-

zone-label-name-pattern*.

Note

tern*")

object-labels "object-name"

tern*))

tern*")

Function

Feature

objects '(object-list))

the face zones of the objects specified.

This requires the volumetric size field

to be computed.

Note

On

object

face

zones

objects "object-name-pat-

tern*")

Note

On

object

face

zones

tern*")

(tgapi-size-field-scale-

geodesic-on-marked-faces

Scales and limits geodesic sizes on the

marked faces for the face zones

On

marked

faces

Scale

geodesic

sizes

'(face-zone-id-list) scale-

factor min-size max-size)

pattern*.

scale-factor min-size max-

size)

Specify the scale-factor.

Specify the values for min-size and

max-size

size)

faces for the face zones specified.

On face

zones

pattern*.

size)

max-size

size)

Function

Feature

faces for the face zone labels specified.

On

object

face

'object-name '(face-zone-la-

face zone labels using a face-zone-

zone

labels

On

object

face

zone

labels

bel-list) scale-factor min-

size max-size)

label-list or face-zone-la-

bel-name-pattern*.

'object-name "face-zone-la-

bel-name-pattern*" scale-

max-size

"object-name" '(face-zone-

label-list) scale-factor

min-size max-size)

"object-name" "face-zone-la-

object face zones specified.

On

object

face

zones

ject-list) '(face-zone-la-

max-size

tern*" scale-factor min-size

max-size)

(tgapi-size-field-filter-

noise-geodesic '(face-zone-

Removes refined surface mesh clusters

generated by geodesic sizing on the

specified face zones.

On face

zones

Filter

noise

id-list) growth-rate face-

count)

pattern*.

name-list) growth-rate face-

count)

noise-geodesic "face-zone-

Specify the growth-rate. It is

recommended to use a growth rate

pattern*.

count)

value higher than the value used for

name-pattern*" growth-rate

face-count)

computing the geodesic sizes (for

example, . ).

Specify the face-count threshold.

For face clusters whose count is less

than the specified threshold value, the

Function

Feature

geodesic size values will be set to the

average of the values on the cluster

boundary.

Note

computed, but

undiffused for the face

zones specified.

(tgapi-size-field-diffuse-

Diffuse geodesic sizing on the specified

face zones. Diffusion can also happen

on face zones which are not specified,

On face

zones

Diffuse

geodesic

sizing

'(face-zone-name-list) min-

if they can be reached by node flood

filling.

size max-size growth-rate

diffuse-across-free-edge?

free-diffusion-range)

pattern*.

'(face-zone-id-list) min-

Specify the minimum and maximum

size limits to apply for the node size

(min-size, max-size.

Important

The sizes will be

bounded to the min-

min-size max-size growth-

rate diffuse-across-free-

edge? free-diffusion-range)

size and max-size

specified. The final

minimum node size

will be the maximum

of (node-min-size,

min-size) and final

maximum node size

will be the minimum

of (node-max-size,

max-size).

It is recommended

that you specify the

global minimum size

required, as you

cannot revert to the

earlier minimum size

after size diffusion.

Function

Feature

Specify the growth-rate to be

applied to diffuse size geodesically

(along the surface).

Choose whether to enable diffusion

of free node sizes to other free nodes

in proximity, even when they are not

connected (set diffuse-across-

free-edge? to #t or #f).

Specify the absolute range to be used

to find free nodes in proximity for

diffusion free-diffusion-range

(when diffuse-across-free-

edge? is enabled (#t).

object labels. Diffusion can also happen

on face zone labels which are not

On

object

face

'object-name '(label-name-

specified, if they can be reached by

node flood filling.

zone

labels

list) min-size max-size

growth-rate diffuse-across-

free-edge? free-diffusion-

range)

Specify the object face zone labels

using the object-name and the

label-name-list or label-

'object-name "label-name-

pattern*" min-size max-size

Important

range)

"object-name" '(label-name-

range)

range)

"object-name" "label-name-

range)

Function

Feature

D.. Examples

Initialize geodesic sizes for the face zones.

(tgapi-size-field-initialize-geodesic-on-face-zones '(inlet1 outlet)

.)

(tgapi-size-field-initialize-geodesic-on-face-zones "part*" .)

Compute the geodesic sizes for curvature size controls.

(tgapi-size-field-compute-geodesic 'curvature*)

Compute the volumetric sizes for BOI size controls.

(tgapi-size-field-compute-volumetric 'boi*)

Compute the geodesic blended size field.

(tgapi-size-field-compute-geodesic-blended '*)

Remove refined surface mesh clusters generated by geodesic sizing on the specified face zones.

(tgapi-size-field-filter-noise-geodesic "part*" . )

Update geodesic sizes with volumetric sizes on selected object face zone labels.

(tgapi-size-field-update-geodesic-with-volumetric-on-face-zones 'part*)

Scale geodesic sizes on marked faces for face zones.

(tgapi-size-field-scale-geodesic-on-marked-faces '(inlet1 outlet) .

. )

Scale geodesic sizes on face zones.

(tgapi-size-field-scale-geodesic-on-face-zones "part*" . . )

Consider a model with objects part1, part2, and part3, inlet1, inlet2, and outlet.

Initialize geodesic sizes for objects.

(tgapi-size-field-initialize-geodesic-on-objects '(inlet1 inlet2 outlet)

.)

(tgapi-size-field-initialize-geodesic-on-objects 'part* .)

Remove refined surface mesh clusters generated by geodesic sizing on the face zones of mesh objects.

(tgapi-size-field-filter-noise-geodesic (get-face-zones-of-objects

(tgapi-util-get-object-name-list-of-type 'mesh)) . )

Update geodesic sizes with volumetric sizes on selected face zones.

(tgapi-size-field-update-geodesic-with-volumetric-on-objects '(inlet1

inlet2 outlet))

Scale geodesic sizes on objects.

(tgapi-size-field-scale-geodesic-on-objects ‘part* . . )

Consider a model with mesh object _fluid with face zone labels part1, part2, and part3, inlet1, inlet2,

and outlet.

Initialize geodesic sizes for object face zone labels.

(tgapi-size-field-initialize-geodesic-on-object-labels ‘_fluid '(inlet1

outlet) .)

(tgapi-size-field-initialize-geodesic-on-object-labels ‘_fluid "part*"

.)

Examples

(tgapi-size-field-update-geodesic-with-volumetric-on-object-labels

'_fluid '(inlet1 outlet))

Scale geodesic sizes on object face zone labels.

(tgapi-size-field-scale-geodesic-on-object-labels '_fluid "part*" .

. )

Appendix E.Wrap Functions

Wrapping functions are available for generating the surface mesh for automotive applications for un-

derhood thermal management (UTM) and external-aero analysis. Note that periodic meshes are not

The following wrap functions are available.

Note

Function

Feature

(tgapi-wrap-objects '(object-

list) 'new-object-name "mater-

ial-point-name" "sizing-type")

Creates the wrapper surface based on the

objects and material point specified. The

wrapper surface creation involves

operations such as Octree creation,

Wrap objects

list) "new-object-name" "mater-

intersection, interface creation, projection

and zone separation.

(tgapi-wrap-objects "object-

name-pattern*" 'new-object-

Specify the objects using an object-

list or object-name-pattern*.

name "material-point-name"

"sizing-type")

Specify a name for the new object.

name-pattern*" "new-object-

Specify the material point ("materi-

al-point-name") to be used for the

wrap operation.

name" "material-point-name"

Specify the sizing type (set "sizing-

type" to "geodesic" or "volumet-

ric".

Note

The size field should be

computed prior to

invoking this API.

(tgapi-wrap-objects-with-seals

object-name-list-or-pattern

Similar to tgapi-wrap-objects with

the addition of seal objects that are used

during interface creation and projection

with seals

'new-object-name "material-

only, in order to prevent leaks. Seal

point-name" "sizing-type"

objects do not participate in imprinting

Function

Feature

and are not associated with the

underlying geometry.

seal-object-name-list-or-pat-

tern)

name (string or symbol) or object-

list (string or symbol) or object-

name-pattern* (string or symbol).

ric".

Note

Specify the seal objects using an ob-

ject-name (string or symbol) or ob-

ric".

Note

ject-list (string or symbol) or ob-

ject-name-pattern* (string or

symbol).

(tgapi-wrap-imprint-object-

features 'mesh-object-name

Imprint feature edges on given mesh

object, and returns feature path extracted

after imprint.

Imprint object

features

separate-off-geometry-edges?

relative-distance critical-

angle)

Specify the mesh object using the

mesh-object-name.

features "mesh-object-name"

Choose whether to delete feature path

edges far from geometry. Set separ-

angle)

ate-off-geometry-edges? to #t

or #f.

Specify the distance tolerance (relat-

ive-distance) and angle tolerance

(critical-angle) to determine the

features far from the geometry, when

is set to #t.

Wrap Functions

Function

Feature

(tgapi-wrap-smooth-face-zones-

with-features-preserved

Smooth face nodes while preserving the

features for the face zones specified.

Face

zones

specified

Smooth

face

nodes

'(face-zone-id-list) mean-

filter-iterations median-fil-

ter-iterations number-of-lay-

ers)

tern*.

Specify the number of mean filter

iterations (mean-filter-itera-

'(face-zone-name-list) mean-

tions). Mean filters use the average of

ers)

adjacent face normal for smoothing.This

method is better for smoothing spikes

ers)

with-features-preserved "face-

Specify the number of median filter

iterations (median-filter-itera-

zone-name-pattern*" mean-fil-

tions). Median filters use the median

ter-iterations median-filter-

iterations number-of-layers)

of adjacent face normal for smoothing.

This method is better for feature

preservation

Specify the number of layers (number-

of-layers) to be smoothed.

Note

You can use the mean

and median filters

individually or use both

together.

(tgapi-wrap-smooth-object-la-

bels-with-features-preserved

features for the object face zone labels

Object

face

zone

labels

specified

'mesh-object-name '(face-zone-

label-list) mean-filter-itera-

tions median-filter-iterations

number-of-layers)

Specify the mesh object and the face

'mesh-object-name "face-zone-

label-name-pattern*" mean-

ers)

"mesh-object-name" '(face-

zone-label-list) mean-filter-

Function

Function

Feature

iterations median-filter-iter-

ations number-of-layers)

"mesh-object-name" "face-zone-

Note

ers)

together.

(tgapi-wrap-smooth-object-off-

geometry-faces 'mesh-object-

name)

Smooth the face nodes of the mesh

object which are far from the geometry.

Specify the mesh object.

Face

nodes

far

from

geometry

geometry-faces "mesh-object-

name")

(tgapi-wrap-separate-object-

face-zones 'mesh-object-name

Separate the mesh object face zones

based on the underlying geometry.

Separate object

face zones

remove-saw-tooth-configura-

tions? saw-tooth-feature-

angle)

Choose whether to remove saw tooth

configurations (set remove-saw-

face-zones "mesh-object-name"

tooth-configurations? to #t or

#f).

angle)

Specify an appropriate value for

saw-tooth-feature-angle.

This is used to identify angle-based

features so as to avoid removal of

saw-tooth configurations, while

separating zones. For example, at

the corner of a cuboid formed by

six planar zones, a corner face is

topologically a saw tooth

configuration, but will not be

rezoned if the saw-tooth-fea-

ture-angle specified is less than

degree. The recommended

range is  to  degrees.

(tgapi-wrap-remesh-object

'mesh-object-name feature-min-

Remesh the mesh object based on the

sizing type specified.

Remesh mesh

object

angle feature-max-angle

corner-angle "sizing-type"

Function

Feature

respect-zone-boundary? front-

Specify the feature-min-angle and

feature-max-angle.The fea-

ture-min-angle and feature-

"mesh-object-name" feature-

max-angle limits are used to retain

angle-based features.The

recommended value for feature-

max-angle is .

ric").

Note

Specify if you want to respect zone

(tgapi-wrap-delete-unwetted-

object-faces 'mesh-object-name

Separate and delete the object faces that

are not in the region of the given material

points.

Delete unwetted

object faces

material-point-name-list-or-

pattern)

points.

pattern)

Specify the objects using a material-

point-name-list or material-

point-name-pattern*.

(tgapi-wrap-resolve-face-inter-

sections-in-object 'mesh-ob-

ject-name)

Resolve face intersections for the mesh

object specified.

Resolve face

intersections

Function

Feature

sections-in-object "mesh-ob-

(tgapi-wrap-inflate-object-

faces-by-dihedral-angle 'mesh-

Inflate mesh object faces based on the

dihedral angle specified.

By

dihedral

angle

Inflate

object

faces

object-name minimum-dihedral-

angle absolute-min-offset rel-

Specify an appropriate value for minim- ative-min-offset number-of-

um-dihedral-angle.The minim-

iterations remove-saw-tooth-

configurations?)

um-dihedral-angle is the angle

faces-by-dihedral-angle "mesh-

between faces connected by an edge.

The faces will be inflated if the angle is

less than the specified value.

object-name" minimum-dihedral-

ative-min-offset number-of-

Specify the absolute-min-offset

and relative-min-offset.

The absolute-min-offset is

the absolute distance used to

move the nodes to increase the

gap. The relative-min-off-

set is the relative distance (as a

factor of local edge length) used

Specify the number of iterations (num-

ber-of-iterations).

#f.

#f.

faces-by-invalid-normal 'mesh-

Inflate mesh object faces based on invalid

normals.

By

invalid

normal

object-name number-of-layers

absolute-min-offset relative-

min-offset number-of-itera-

Specify an appropriate value for num-

ber-of-layers.The number-of-

tions remove-saw-tooth-config-

urations?)

layers is the number of layers of face

nodes around the invalid normal

location to be inflated.

object-name" number-of-layers

Function

Feature

#f.

(tgapi-wrap-improve-object-

quality 'mesh-object-name ag-

gressively?)

Improve the mesh object quality.

Improve

mesh

object

quality

Improve

mesh

object

quality "mesh-object-name"

aggressively?)

Enable aggressive improvement if

required (set aggressively? to #t

or #f.When this option is enabled, the

features may not be preserved during

the improve operation.

for-tet-meshing 'mesh-object-

Improve mesh object for tet meshing.

For tet

meshing

max-cell-skewness max-face-

skewness max-face-size-change)

al-point-name").

for-tet-meshing "mesh-object-

Set the max-cell-skewness, max-

face-skewness, and max-face-

size-change.

for-prism-meshing 'mesh-ob-

Improve mesh object for prism meshing.

In general, zones will inherit the prism

settings from the underlying geometry.

For

prism

meshing

ject-name number-of-layers

For zones that do not inherit prism

"offset-method" prism-aspect-

settings, the settings passed as arguments

will be used.

ratio last-ratio-percentage

prism-layer-first-height

prism-layer-growth-rate qual-

ity-measure max-cell-skewness

max-face-skewness keep-

prisms?)

of-layers).The number of layers

for-prism-meshing "mesh-ob-

should be the same as that set for prism

meshing.

ject-name" number-of-layers

Set the prism offset-method. Select

one of the options "aspect-ratio",

offset-method prism-aspect-

Function

Feature

"last-ratio", "uniform", or

"minimum-height".

Set the prism-aspect-ratio, if

applicable.

Feature

prisms?)

Set the last-ratio-percentage,

Set the prism-layer-first-

height.

Set the prism-layer-growth-

rate.

Specify the quality-measure to be

used.

Set the max-cell-skewness and

max-face-skewness.

Choose whether to retain the prisms (set

keep-prisms? to #f or #t) (setting

to #t requires beta features to be

enabled).

Note

A value of - can be used

for the parameters that

are not required for a

particular offset method.

E.. Examples

For a model with geometry objects part1, part2, part3 and material point fluid:

Compute the size field.

Wrap the geometry objects using the material point fluid.

(tgapi-wrap-objects 'part* '_fluid "fluid" "geodesic")

Imprint feature edges on the mesh object.

(tgapi-wrap-imprint-object-features '_fluid #t . )

Smooth face nodes while preserving features.

(tgapi-wrap-smooth-face-zones-with-features-preserved (get-face-zones-

of-objects '(_fluid))   )

Smooth the face nodes of the mesh object which are far from the geometry.

(tgapi-wrap-smooth-object-off-geometry-faces '_fluid)

Remesh the mesh object.

(tgapi-wrap-remesh-object '_fluid . . . "geodesic" #f .)

(tgapi-wrap-improve-object '_fluid #t)

Resolve thin regions and self intersections.

(tgapi-wrap-inflate-object-faces-by-invalid-normal '_fluid  . .

#t)

(tgapi-wrap-inflate-object-faces-by-dihedral-angle '_fluid  . .

#t)

(tgapi-wrap-resolve-face-intersections-in-object '_fluid)

#t)

#t)

(tgapi-wrap-improve-object-for-tet-meshing '_fluid "fluid" . . .)

(tgapi-wrap-improve-object-for-prism-meshing '_fluid  "aspect-ratio"

- . "inverse-ortho" . . #f)

Note

A value of - has been used for the parameters that are not required for the offset

method chosen.

Remove unwetted object faces.

(tgapi-wrap-delete-unwetted-object-faces ‘wrap-v2 ‘ext*)

(tgapi-wrap-delete-unwetted-object-faces “wrap-v2” (list “external”

“mat-pt1”))

(tgapi-wrap-delete-unwetted-object-faces “wrap-v2” “mat-pt1”)

Separate the mesh object face zones based on the geometry.

(tgapi-wrap-separate-object-face-zones '_fluid #t .)

Examples

The section describes the text command listing for Fluent in Solution mode.

adapt/ (p. ) lists commands related to mesh adaption.

adjoint/ (p. ) lists commands related to the adjoint solver.

define/  (p. ) lists commands related to problem definition, such as models, boundary conditions, ma-

terials, etc.

display/  (p. ) lists commands used to control the rendering of your model and mesh in the graphical

window.

exit / close-fluent (p. ) lists the command to close the program.

mesh/ (p. ) lists commands used to create and manage mesh properties.

parallel/  (p. ) lists commands specific to parallel processing.

plot/  (p. ) lists commands specific to plotting data.

report/  (p. ) lists commands used to return statistics for the simulation.

server/  (p. ) lists commands used control the Fluent Remote Visualization Client and Server.

solve/  (p. ) lists commands used to create and manage solution controls, such as animation, cell registers,

monitors, initialization, etc.

surface/ (p. ) lists commands related to creating and manipulating surfaces.

switch-to-meshing-mode (p. ) lists the command to transfer your solution data to Fluent in meshing

mode.

turbo/ (p. ) lists commands related to results and reporting for turbomachinery.

views/ (p. ) lists commands related to camera and view manipulation in the graphics window.

battery-model/ (p. ) lists commands related to battery models.

Fuel Cell Text Commands (p. ) lists commands related to fuel cell models.

Fuel Cell Text Commands (p. ) lists commands related to magnetohydrodynamics models.

Chapter : adapt/

Important

The adapt/ text command menu is only available if you have used the following text

command: mesh/adapt/revert-to-R19.-user-interface. Accessing the adapt/

text command menu in this way will not be possible in future releases.

adapt-boundary-cells

Adapts boundary cells based on a list of face zones.

adapt-to-gradients

Adapts mesh based on the gradient adaption function from the selected scalar quantity, the adaption

threshold values, and the adaption limits.

adapt-to-ref-lev

Adapts cells based on refinement level differences.

adapt-to-register

Adapts mesh based on the selected register and adaption limits.

adapt-to-vol-change

Adapts cells with large changes in cell volume.

adapt-to-volume

Adapts cells that are larger than a prescribed volume.

adapt-to-y+

Adapts cells associated with all wall zones based on the specified threshold values and adaption limits.

adapt-to-y+-zones

Adapts cells associated with specified wall zones based on the specified threshold values and adaption

limits.

anisotropic-adaption

Anisotropically refines boundary layers. Cells will be split in the normal direction to the boundary face.

adapt-to-y*

adapt-to-y*-zones

limits.

change-register-type

Toggles specified register between refinement and mask.

combine-registers

Combines the selected adaption and/or mask registers to create hybrid adaption functions.

delete-register

Deletes a register.

display-register

Displays the cells marked for adaption in the specified register.

exchange-marks

Exchanges the refinement and coarsening marks of the specified register.

fill-crsn-register

Marks all cells to coarsen that are not marked for refinement in the register.

free-parents

Deletes the hanging node face and cell hierarchy.

free-registers

Deletes all adaption and mask registers.

invert-mask

Changes all the active cells to inactive cells in a mask register.

limit-register

Applies the adaption volume limit to the selected register.

list-registers

Prints a list of the current registers including the ID, description (name), number of cells marked for refine-

ment and coarsening, and the type.

mark-boundary-cells

Marks boundary cells based on a list of zones for refinement.

mark-boundary-normal

Marks cells for refinement based on target boundary normal distance.

mark-boundary-vol

Marks cells for refinement based on target boundary volume.

mark-inout-circle

Marks cells with centroids inside/outside the circular region defined by text or mouse input.

mark-inout-cylinder

Marks cells with centroids inside/outside the arbitrarily oriented cylindrical region defined by text or mouse

input.

mark-inout-hexahedron

Marks cells with centroids inside/outside the hexahedral region defined by text or mouse input.

mark-inout-iso-range

Marks cells for refinement that have values inside/outside the specified isovalue ranges of the selected

field variable.

adapt/

mark-inout-rectangle

Marks cells with centroids inside/outside the rectangular region defined by text or mouse input.

mark-inout-sphere

Marks cells with centroids inside/outside the spherical region defined by text or mouse input.

mark-percent-of-ncells

Marks percent of total cell count for adaption based on gradient or isovalue.

mark-with-gradients

Marks cells for adaption based on flow gradients for refinement.

mark-with-ref-lev

Marks cells based on refinement level differences.

mark-with-vol-change

Marks cells with large changes in cell volume for refinement.

mark-with-volume

Marks cells for adaption based on maximum allowed volume.

mark-with-y+

Marks cells associated with all wall zones for refinement or coarsening based on the specified threshold

values.

mark-with-y+-zones

values.

Marks only cells associated with specified wall zones for refinement or coarsening based on the specified

threshold values.

mark-with-y*

values.

mark-with-y*-zones

set/

Enters the adaption set menu.

cell-zones

Sets cell zones to be used for marking adaption.

coarsen-mesh?

Turns on/off ability to coarsen mesh.

display-crsn-settings

Prompts for coarsening wireframe visibility and shading, and the marker visibility, color, size and

symbol.

display-node-flags

Displays s color coded markers at the nodes specifying the node type.

display-refn-settings

Prompts for refinement wireframe visibility and shading, and the marker visibility, color, size and

symbol.

grad-vol-weight

Controls the volume weighting for the gradient adaption function.

init-node-flags

Initializes the node flags.

max-level-refine

Sets maximum level of refine in the mesh.

max-number-cells

Limits the total number of cells produced by refinement.

method

Sets the adaption method.

min-cell-quality

Sets the minimum value allowed for the orthogonal quality of cells during adaption. If your solution

diverges, you may find that using a higher minimum quality value resolves the issue.This text command

is only available for PUMA 3D adaption (that is, when you have entered adapt/set/method ).

min-cell-volume

Restricts the size of the cells considered for refinement.

min-number-cells

Sets limit on the number of cells in the mesh.

reconstruct-geometry

Enables/disables geometry-based adaption.

refine-mesh?

Turns on/off mesh adaption by point addition.

set-geometry-controls

Sets geometry controls for wall zones.

verbosity

Allows to set the adaption verbosity.

smooth-mesh

Smoothes the mesh using the quality-based, Laplacian, or skewness methods.

swap-mesh-faces

Swaps the faces of cells that do not meet the Delaunay circle test.

adapt/

Chapter : adjoint/

controls/

Menu to configure adjoint solver controls.

settings

Sets parameters for the adjoint solver numerics.

stabilization

Sets parameters for the adjoint stabilization schemes.

stabilization-strategy

Enters the stabilization strategy menu, where you can define the stabilization strategy and settings

for the adjoint solver.

complex-case-settings

Defines the settings that are recommended for complex cases.

default-settings

Defines settings that are recommended for standard cases.These settings are used by default.

settings

Allows you to define a custom settings.

type

Allows you to define the stabilization strategy type.

design-tool/

Enters the design-tool menu.

design-change/

Performs optimal shape modification.

calculate-design-change

Computes the optimal design change.

check

Prints a report in the console that summarizes the control points defined for the region, the defined

constraining and/or deformation conditions, and any possible conflicts between multiple constraints

/ deformations applied on a single node.

display-applied-conditions

Displays all of the applied conditions in the graphics window, each type in a unique color. Note

that this includes the selected design conditions, as well as the fixed conditions applied to zones

that are not selected for deformation.

export-displacements

Exports the computed optimal displacements.

export-stl

Exports specified surfaces from 3D cases as an .stl file.

modify-mesh

Applies the computed optimal displacement to the mesh.

multiobjective-weights

Sets the weights for multiple free-form objectives.

preview-mesh

Displays the planned changes in the graphics window for select surfaces (undeformed in white,

deformed in green).

print-expected-changes

Prints the expected changes.

revert-mesh

Reverts (rejects) the last mesh modification.

select-conditions

Selects which conditions to apply to the mesh deformation.

select-morphing-method

Selects the morphing method.

select-strict-conditions

Selects constraining and/or deformation conditions you want strictly enforced (that is, applied to

all of the nodes of the associated zones).

select-zones

Selects which zones are allowed to deform.

settings

Specifies global deformation scale and settings.

write-expected-changes

Writes out the expected changes in the observables for the computed optimal design change.

design-conditions/

Creates, deletes, displays (with various options), renames, and/or sets conditions on the geometry

numerics

Adjusts numerics settings for computing the optimal displacement.

objectives/

Menu to configure observable objectives.

include-current?

numerics

Optionally includes the most-recently computed observable sensitivity in the multi-objective design

computation.

manage/

Menu to import, export, and manage sensitivity data.

adjoint/

set

Configures the objectives for loaded observables.

region-conditions/

Menu to configure conditions on the deformation region

Specifies what degree of continuity to enforce at the boundaries of the deformation region.

motion

Specifies conditions on the movement of the control points.

points

Specifies the number of control points in the deformation region.

symmetry

Specifies symmetry conditions for the deformation region.

region/

Menu to define the deformation region.

cartesian-limits

Directly specifies the bounds of the Cartesian deformation region.

cylindrical-limits

Directly specifies the bounds of the cylindrical deformation region.

export-sensitivities

Exports the sensitivity to mesh node movement for the currently selected observable. Sensitivities

are only exported for mesh nodes that lie within the specified deformation region.

get-bounds

Sets the limits for the deformation region to encompass a list of selected surfaces.

larger-box

Uniformly increases the size of the deformation region.

set-region-type

Specifies whether the deformation region is either a Cartesian or cylindrical region type.

smaller-box

Uniformly decreases the size of the deformation region.

expert/

Provides text commands that allow you to undo enhancements to the default adjoint solver behavior.

undo-2019r3-default-changes?

expert/

Allows you to undo an enhancement introduced in version  R3 of ANSYS Fluent: the use of a full

(rather than a flexible) cycle algebraic multigrid (AMG) solver in the adjoint solver, which can improve

convergence and efficiency.

undo-r19.-default-changes?

Allows you to undo enhancements introduced in version . of ANSYS Fluent, including a modified

Rhie-Chow averaging method (to be consistent with default changes introduced in the general solver

in version . ), a non-conservative form of the adjoint equations, an enhanced method for building

the algebraic multigrid (AMG) matrix for the adjoint solver, and a disabling of the early protection

scheme used by the AMG solver for the adjoint calculations.

methods/

Menu to configure adjoint solver settings.

settings

Defines settings such as spatial discretization methods for the adjoint solver.

Applies defaults to adjoint solver settings such as spatial discretization methods.

best-match-settings

Defines settings such as spatial discretization methods for the adjoint solver to match those for the

flow solver as closely as possible.

monitors/

Menu to configure monitors for the adjoint solver.

plot-residuals

Plots the adjoint residuals in the designated graphics window.

settings

Allows you to configure the monitors and convergence criteria for the adjoint solver.

observable/

Menu to create and configure observables of interest.

create

A new observable of the specified type and name is created and the definition is populated with default

delete

Removes a named observable.

create

delete

evaluate

Evaluates the current value of the selected observable and prints the result to the console.

rename

An existing observable is renamed to a new specified name.

select

A named observable is selected as the one for which an adjoint solution is to be computed.

specify

The parameters that define a named observable are configured.

write

Evaluates the current value of the selected observable and writes the result to a file.

optimizer/

Enters the optimizer menu, where you can use a gradient-based optimizer to optimize the geometry to

meet multiple goals for multiple observables at multiple operating conditions.

adjoint/

calculate\

Enters the calculate menu, for running the adjoint-based optimizer.

Initializes the optimizer and clears out the optimization history.

optimize

Runs adjoint-based optimization.

reset

Sets the current design iteration as the optimal solution.

summarize

Reports the optimization history.

calculation-activities/

Enters the calculation-activities menu, for setting activities during the adjoint optimization.

animate/

Enters the animate menu, for outputting plots for animations every design iteration.

define/

Enters the animation definition menu.

define-monitor

Defines new animation.

edit-monitor

Change animation monitor attributes.

objects/

Enters the objects menu to define, edit, delete solution animation objects.

clear-history

Clears object history.

copy

Copies graphics object.

create

Creates new graphics object.

delete

Deletes graphics object.

edit

Edits graphics object.

playback/

Enters the animation playback menu.

delete

copy

create

delete

edit

playback/

delete

Deletes animation sequence.

play

Plays the selected animation.

read

Reads new animation from file or already-defined animations.

stored-view?

Plays the 3D animation sequence using the view stored in the sequence.

write

Writes animation sequence to the file.

auto-save

Saves files every design iteration.

execute-commands/

Enters the execute-monitor-commands menu.

add-edit

Adds or edits execute-commands.

disable

Disables an execute-command.

enable

Enables an execute-command.

monitor

Monitors the adjoint optimization.

plot

Plots monitors.

settings

Settings for monitors.

mesh-quality\

Enters the mesh-quality menu, for printing and setting the requirement of mesh quality during the

adjoint optimization.

mesh-quality-settings

Sets the requirement of mesh quality during the adjoint optimization.

print-current-status

Prints the current mesh quality status.

optimizer-objectives/

Enters the optimizer-objectives menu, for setting the objectives in the adjoint optimizer.

set-adaptive-change

Sets adaptive change.

set-conditions

Sets operating conditions.

adjoint/

set-objectives

Sets multi-objectives.

set-observables

Choose observables.

optimizer-settings

Sets the settings in the adjoint optimizer.

reporting/

Menu to report sensitivity data from the adjoint solution.

report

Reports sensitivity data on a named flow boundary.

write

Reports sensitivity data on a named flow boundary and writes it to a named file.

run/

Menu to initialize and compute the adjoint solution.

Initializes the adjoint solution field to zero everywhere.

run/

initialize-stabilization

Initializes the stabilization data.This text command is only available if the residual minimization or

modal stabilization is used.

initialize-strategy

Initializes the stabilization strategy, such that the first stabilization scheme is used at the start of the

next calculation rather than continuing to use the second stabilization scheme.This text command is

only available when the blended stabilization strategy is used.

iterate

Advances the adjoint solver by a specified number of iterations, or until the convergence criteria are

met.

Chapter : define/

Enters the boundary conditions menu.

Important

Text User Interface commands that take single or multiple zone names support the use

of wildcards. For example, to copy boundary conditions (copy-bc) to all zones of a

certain type, use a * in the name of the zone to which you want to copy the conditions.

axis

Sets boundary conditions for a zone of this type.

bc-settings/

Enters the boundary conditions settings menu.

mass-flow

Selects method for setting the mass flow rate.

Sets advanced options for pressure outlet boundaries.

copy-bc

Copies boundary conditions to other zones.

degassing

fan

fluid

interface

interior

interface

interior

list-zones

Prints out the types and IDs of all zones in the console window.You can use your mouse to check a

zone ID, following the instructions listed under Zone in the Boundary Conditions Task Page  section

of the User’s Guide.

modify-zones/

Enters the modify zones menu.

activate-cell-zone

Activates cell thread.

Appends new mesh.

append-mesh-data

Appends new mesh with data.

change-zone-state

Sets the state (liquid or vapor) for a specific fluid zone.

copy-move-cell-zone

Creates a copy of a cell zone that is offset from the original either by a translational distance or a

rotational angle. In the copied zone, the bounding face zones are all converted to walls, any existing

cell data is initialized to a constant value, and non-conformal interfaces and dynamic zones are

not copied; otherwise, the model settings are the same as in the original zone. Note that if you

want the copied zone to be connected to existing zones, you must either fuse the boundaries (see

Fusing Face Zones in the Fluent User's Guide) or set up a non-conformal interface (see Using a Non-

Conformal Mesh in ANSYS Fluent in the Fluent User's Guide).

copy-mrf-to-mesh-motion

Copies motion variable values for origin, axis, and velocities from Frame Motion to Mesh Motion.

copy-mesh-to-mrf-motion

Copies motion variable values for origin, axis, and velocities from Mesh Motion to Frame Motion.

create-all-shell-threads

Marks all finite thickness walls for shell creation. Shell zones will be created at the start of the iter-

ations.

create-periodic-interface

Creates a conformal or non-conformal periodic interface.

deactivate-cell-zone

Deactivates cell thread.

define/

delete-all-shells

Deletes all shell zones and switches off shell conduction on all the walls.These zones can be recre-

ated using the command recreate-all-shells.

delete-cell-zone

Deletes a cell thread.

extrude-face-zone-delta

Extrudes a face thread a specified distance based on a list of deltas.

extrude-face-zone-para

Extrudes a face thread a specified distance based on a distance and a list of parametric locations

between  and , for example,  . . . ..

fuse-face-zones

Attempts to fuse zones by removing duplicate faces and nodes.

Lists zone IDs, types, kinds, and names.

Attempts to establish periodic/shadow face zone connectivity.

matching-tolerance

Sets normalized tolerance used for finding coincident nodes.

merge-zones

Merges zones of same type and condition into one.

mrf-to-sliding-mesh

Changes the motion specification from MRF to moving mesh.

orient-face-zone

Orients the face zone.

recreate-all-shells

Recreates shells on all the walls that were deleted using the command delete-all-shells.

replace-zone

Replaces cell zone.

sep-cell-zone-mark

Separates cell zone based on cell marking.

sep-cell-zone-region

Separates cell zone based on contiguous regions.

sep-face-zone-angle

Separates face zone based on significant angle.

sep-face-zone-face

Separates each face in zone into unique zone.

sep-face-zone-mark

Separates face zone based on cell marking.

sep-face-zone-region

Separates face zone based on contiguous regions.

slit-periodic

Slits periodic zone into two symmetry zones.

slit-face-zone

Slits two-sided wall into two connected wall zones.

slit-interior-between-diff-solids

Slits the interior zone between solid zones of differing materials to create a coupled wall.You will

generally be prompted by Fluent if this is necessary.

zone-name

Gives a zone a new name.

zone-type

Sets the type for a zone or multiple zones of the same category.You will be prompted for the name

/ ID of the zone to be changed and the new type for that zone.To change multiple zones, you can

enter a list (separated by spaces and contained within a pair of parentheses) or use asterisks (*) as

wildcards.

non-overlapping-zone-name

Displays the name of the non-overlapping zone associated with a specified interface zone.This text

command is only available after a mesh interface has been created.

non-reflecting-bc/

Enters the non-reflecting boundary condition menu.

general-nrbc/

Setting for general non-reflecting b.c.

set/

Enters the setup menu for general non-reflecting b.c.’s.

sigma

Sets NRBC sigma factor (default value . ).

sigma2

Sets NRBC sigma2 factor (default value . ).

verbosity

Enables/disables nrbc verbosity scheme output.

turbo-specific-nrbc/

Enters the turbo specific nrbc menu.

enable?

Enables/disables non-reflecting b.c.’s.

Initializes non-reflecting b.c.’s.

set/

Enters the set menu for non-reflecting b.c. parameters.

define/

enable?

set/

define/

Enables use of higher-order reconstruction at boundaries if available.

Sets non-reflecting b.c. under-relaxation factor.

verbosity

Sets non-reflecting b.c. verbosity level. : silent,  : basic information (default),  : detailed

information for debugging.

show-status

Shows current status of non-reflecting b.c.’s.

open-channel-wave-settings

Opens channel wave input analysis.

openchannel-threads

Lists open channel group IDs, names, types and variables.

outflow

periodic

phase-shift/

Enters the phase shift settings menu.

multi-disturbances

Sets basic phase-shift parameters.

extra-settings

Sets other phase-shift parameters.

radiator

rans-les-interface

recirculation-inlet

recirculation-outlet

set/

Allows you to define one or more settings at single or multiple boundaries/cell zones of a given type

at once. Enters q to exit the define/boundary-conditions/set/<type>  command.

set/

For a description of the items in this menu, see corresponding define/boundary-condi-

tions/<type> .

shadow

solid

symmetry

target-mass-flow-rate-settings/

Enters the targeted mass flow rate settings menu.

set under-relaxation-factor

The default setting is ..

enable targeted mass flow rate verbosity?

Enables/disables verbosity when using targeted mass flow rate.When enabled, it prints to the

console window the required mass flow rate, computed mass flow rate, mean pressure, the new

pressure imposed on the outlet, and the change in pressure in SI units.

wall

zone-name

zone-type

Sets the type for a zone or multiple zones of the same category.You will be prompted for the name /

ID of the zone to be changed and the new type for that zone.To change multiple zones, you can enter

a list (separated by spaces and contained within a pair of parentheses) or use asterisks (*) as wildcards.

custom-field-functions/

Enters the custom field functions menu.

define

Defines a custom field function.

delete

Deletes a custom field function.

define/

example-cff-definitions

Lists example custom field functions.

list-valid-cell-function-names

Lists the names of cell functions that can be used in a custom field function.

load

Loads a custom field function.

save

load

save

Saves a custom field function.

dynamic-mesh/

Enters the dynamic mesh menu.

actions/

Enters the dynamic mesh action menu, where you can initiate manual remeshing (that is, remeshing

without running a calculation).

remesh-cell-zone

Manually remeshes a cell zone with option to remesh adjacent dynamic face zones.

remesh-cell-zone-cutcell

Manually remeshes a cell zone using the CutCell zone remeshing method, in order to generate a

predominantly Cartesian mesh.

controls/

Enters the dynamic mesh controls menu.This text command is only available when the define/dy-

namic-mesh/dynamic-mesh? text command is enabled.

contact-parameters/

Enters the dynamic mesh contact-parameters menu.This text command is only available when

you enable contact detection using the prompts of the define/dynamic-mesh/dynamic-

mesh? text command.

contact-threshold

Specifies threshold distance for contact detection.

contact-udf

Selects the UDF to be invoked when contact is detected.

contact-zones

Selects face zones involved in contact detection.

flow-control?

Enables/disables flow control.

flow-control-parameters/

Sets up and deletes flow control zones

create-flow-control-zone

Creates a flow control zone.

delete-flow-control-zone

Deletes a flow control zone.

implicit-update-parameters/

Enters the dynamic mesh implicit update menu.This text command is only available when you

enable implicit mesh updating using the prompts of the define/dynamic-mesh/dynamic-

motion-relaxation

Specifies a value (within the range of  to ) for the motion relaxation, which is applied during

the implicit mesh update.

residual-criteria

Specifies the relative residual threshold that is used to check the motion convergence during

update-interval

Specifies the update interval (that is, the frequency in iterations) at which the mesh is updated

within a time step.

in-cylinder-output?

Enables/disables in-cylinder output.

in-cylinder-parameters/

Enters the dynamic mesh in-cylinder menu.

crank-angle-step

Specifies crank angle step size.

crank-period

Specifies the crank period.

max-crank-angle-step

Specifies maximum crank angle step size.

minimum-lift

Specifies minimum lift for in-cylinder valves.

modify-lift

Modifies lift curve (shift or scale).

piston-data

Specifies the crank radius and connecting rod length.

piston-stroke-cutoff

Specifies the cut off point for in-cylinder piston.

position-starting-mesh

Moves mesh from top dead center to starting crank angle.

print-plot-lift

Prints or plot valve lift curve.

starting-crank-angle

Specifies the initial value for the crank angle.

layering?

Enables/disables dynamic-layering in quad/hex cell zones.

define/

layering-parameters/

Enters the dynamic mesh layering menu.

collapse-factor

Sets the factor determining when to collapse dynamic layers.

constant-height?

Enables/disables layering based on constant height, else layering based on constant ratio.

split-factor

Sets the factor determining when to split dynamic layers.

remeshing?

Enables/disables local remeshing in tri/tet and mixed cell zones.

remeshing-parameters/

Enters the dynamic mesh remeshing menu to set parameters for all remeshing methods except

the Cutcell zone remeshing method.

cell-skew-max

Sets the cell skewness threshold above which cells will be remeshed.

face-skew-max

Sets the face skewness threshold above which faces will be remeshed.

length-max

Sets the length threshold above which cells will be remeshed.

length-min

Sets the length threshold below which cells will be remeshed.

Enables/disables cavity replacement only if remeshing improves the skewness.

parallel-remeshing?

Disables/enables parallel remeshing.

remeshing-after-moving?

Enables a second round of remeshing based on the skewness parameters after the boundary

has moved.

remeshing-methods

Enables/disables remeshing methods.

size-remesh-interval

Sets the interval (in time steps) when remeshing based on size is done.

sizing-funct-defaults

Sets sizing function defaults.

sizing-funct-rate

Determines how far from the boundary the increase/decrease happens.

sizing-funct-resolution

Sets the sizing function resolution with respect to shortest boundary.

sizing-funct-variation

Sets the maximum sizing function increase/decrease in the interior.

sizing-function?

Enables/disables sizing function to control size based remeshing.

six-dof-parameters/

Enters the dynamic mesh six degrees of freedom (DOF) solver menu.

create-properties

Creates/edits a set of six DOF properties for rigid body motion.

delete-properties

Deletes a set of six DOF properties for rigid body motion.

list-properties

Prints summaries of the existing sets of six DOF properties for rigid body motion.

motion-history-file-name

Specifies the name and location of the six DOF motion history file.

motion-history?

Enables/disables writing position/orientation of six DOF zones to file.

second-order?

Enables/disables the second order six degrees of freedom solver.

x-component-of-gravity

Specifies x-component of gravity.

y-component-of-gravity

Specifies y-component of gravity.

z-component-of-gravity

Specifies z-component of gravity.

smoothing?

Enables/disables smoothing in cell zones.

smoothing-parameters/

Enters the dynamic mesh smoothing menu.

amg-stabilization

Sets the algebraic multigrid (AMG) stabilization method for mesh smoothing calculations that

use finite element discretization.

bnd-node-relaxation

The boundary node relaxation is used by spring smoothing.The boundary node relaxation allows

you to relax the update of the node positions at deforming boundaries. A value of  prevents

deforming boundary nodes from moving and a value of  indicates no under-relaxation.

bnd-stiffness-factor

Sets the stiffness factor for springs connected to boundary nodes.

define/

boundary-distance-method

Sets the method used to evaluate the boundary distance for the diffusion coefficient calculation,

when diffusion-based smoothing is enabled.

constant-factor

Sets the spring constant relaxation factor.

convergence-tolerance

Sets the convergence tolerance for spring-based solver.

diffusion-coeff-function

Specifies whether the diffusion coefficient for diffusion-based smoothing is based on the

boundary distance or the cell volume.

diffusion-coeff-parameter

Sets the diffusion coefficient parameter used for diffusion-based smoothing.

diffusion-fvm?

Answering yes at the prompt changes the diffusion-based smoothing method to the cell-

based finite volume approach that was the default in releases prior to Fluent .. Answering

no at the prompt changes the diffusion-based smoothing method to the default node-based

finite element method.

max-iter

Sets the maximum number of iterations for the smoothing calculations.

relative-convergence-tolerance

Sets the relative residual convergence tolerance for smoothing based on diffusion or the linearly

elastic solid model.

skew-smooth-cell-skew-max

Sets the skewness threshold, above which cells will be smoothed using the skewness method.

skew-smooth-face-skew-max

Sets the skewness threshold, above which faces will be smoothed using the skewness method.

skew-smooth-niter

Sets the number of skewness-based smoothing cycles.

smooth-from-reference-position?

Enables/disables smoothing from a reference position. Such smoothing may produce greater

mesh quality consistency for stationary or moving meshes with periodic or quasi-periodic

motion, and is only available when the smoothing method is based on diffusion or the linearly

smoothing-method

Specifies the smoothing method (spring, diffusion, or linearly elastic solid) used by the dynamic

mesh model.

spring-on-all-elements?

Enables/disables spring-based smoothing for all cell shapes; if disabled, the spring-based

smoothing is applied based on the setting of the define/dynamic-mesh/con-

trols/smoothing-parameters/spring-on-simplex-shapes? text command.

spring-on-simplex-shapes?

Enables/disables spring-based smoothing for triangular / tetrahedral cells in mixed element

zones; if disabled, the spring-based smoothing is applied to triangular / tetrahedral cells in

triangular / tetrahedral element zones.

poisson-ratio

Sets the Poisson’s ratio used for smoothing based on the linearly elastic solid model.

verbosity

Setting this to  will cause smoothing residuals to be printed to the text console.The default

value of  suppresses this output.

dynamic-mesh?

Enables/disables the dynamic mesh solver.

events/

Enters the dynamic mesh events menu.

export-event-file

Exports dynamic mesh events to file.

import-event-file

Imports dynamic mesh event file.

steady-pseudo-time-control

Enables/disables the pseudo time step control in the graphical user interface.

transient-settings/

Enters the transient dynamic mesh settings menu.This text command is only available when you enable

dynamic mesh using the prompts of the define/dynamic-mesh/dynamic-mesh? text command.

Solver time must also be set to Transient.

allow-second-order?

Enables/disables second order transient scheme for dynamic mesh cases.

verbosity

Enables/disables transient scheme verbosity for dynamic mesh cases.

zones/

Enters the dynamic mesh zones menu.

create

Creates or edit a dynamic zone.

delete

Deletes a dynamic zone.

insert-boundary-layer

Inserts a new cell zone.

insert-interior-layer

Inserts a new layer cell zone at a specified location.

list

delete

list

Lists the dynamic zones.

define/

remove-boundary-layer

Removes a cell zone.

remove-interior-layer

Removes an interior layer cell zone.

enable-mesh-morpher-optimizer?

Enables the mesh morpher/optimizer.When the mesh morpher/optimizer is enabled, the define/mesh-

morpher-optimizer text command becomes available.

injections/

Enters the injections menu.

For a description of the items in this menu, see define/models/dpm/injections.

materials/

Enters the materials menu.

change-create

Changes the properties of a locally-stored material or create a new material.

copy

Copies a material from the database.

copy-by-formula

Copies a material from the database by formula.

data-base/

Enters the material database menu.

database-type

Sets the database type.

edit

Edits material.

list-materials

Lists all materials in the database.

Lists the properties of a material in the database.

new

Defines new material.

save

Saves user-defined database.

delete

Deletes a material from local storage.

Lists all locally-stored materials.

Lists the properties of a locally-stored material.

mesh-interfaces/

Enters the mesh-interfaces menu.

auto-options/

Enters the auto-options menu.

proximity-tolerance

Sets the tolerance used when automatically grouping zones to create one-to-one mesh interfaces.

The proximity tolerance is defined relative to the edge lengths in the interface zones, and can

range from  to  (representing the minimum and maximum edge lengths, respectively).

auto-pairing

Creates mesh interfaces for some or all of the interface zones.This text command automatically "pairs"

the zones, so that you do not have to manually assign the zones to the two sides of each interface as

part of the creation process. Note that not all of the interface options are available at the time of creation:

some can be enabled afterward using the define/mesh-interfaces/edit text command; for

the periodic and periodic repeats options, you must instead create the interface using the

define/mesh-interfaces/make-periodic and define/mesh-interfaces/create text

commands, respectively.

create

Creates a mesh interface.

delete

Deletes a mesh interface.

Deletes all sliding-interfaces.

draw

Draws specified sliding interface zone.

edit

Edits attributes of mesh interfaces, including the interface options and (for a single interface) the name

and the list of interface zones assigned to the interface.

enforce-continuity-after-bc?

Enables/disables continuity across the boundary condition interface for contour plots in postprocessing.

enforce-coupled-wall-between-solids?

Enables/disables automatic definition of solid-solid interfaces as coupled walls. By default this option

is disabled and ANSYS Fluent creates interior boundaries at solid-solid interfaces.

improve-quality

Checks the quality of all mapped interfaces. If Fluent finds any mapped interfaces that require improve-

ment it will list them and ask you if you would like to increase the tolerance to improve the interfaces.

list

Lists all mesh interfaces.

define/

list

define/

Makes interface zones periodic.

mapped-interface-options/

Enters the mapped-interface menu. Options are available to convert a non-conformal interface to a

mapped interface.

convert-to-mapped-interface

Converts non-conformal mesh interface to mapped mesh interfaces. Answering yes to

Convert all mesh interfaces to mapped mesh interfaces? will enforce

the mapping such that it specifies all interfaces as mapped interfaces; the mapped interfaces

are created regardless of mesh quality. Answering yes to Convert poorly matching

mesh interfaces to mapped mesh interfaces? will automate the mapping

such that all interfaces that penetrate each other are automatically defined as mapped in-

terfaces. Note that in all cases, only interfaces for which at least one side of the interface

consists of only solid zones will be converted.

tolerance

Specifies the mapped interface tolerance. After changing the tolerance, the existing mapped inter-

face will be updated.

solution-controls

Specifies the mapped frequency and under-relaxation factor for mapped interfaces.

mapped-interface-solution-controls

Sets the mapping frequency and under-relaxation factor.

mapped-interface-tolerance

Specifies the tolerance for creating mapped interfaces.

non-conformal-interface-numerics/

Enters the non-conformal-interface-numerics menu.

change-numerics?

Provides options to improve numerics for non-conformal interfaces in some cases.

Enforce watertight cells for fluid-solid and solid-solid inter-

faces? : Answering yes ensures cells adjacent to a non-conformal fluid-solid or solid-

solid interface are watertight when performing the coupled wall discretization.

Use enhanced gradient computations for fluid-solid and solid-

solid interfaces? : Answering yes enables improvements to the calculation of

gradients.

Recreate non-conformal interfaces? : If you change the response to either of

the previous two questions then interfaces should be recreated.

transfer-motion-across-interfaces?

Enables/disables the automatic transfer of motion across a mesh interface when only one side is

moving as a result of user-defined or system coupling motion.You can specify the method by which

the motion is transferred: transfer-displacements (the default) interpolates nodal displacement

from the active side of the interface to the passive side, and is recommended when there are gaps

and/or penetrations in the mesh interface that must be maintained; project-nodes projects the

passive nodes onto the faces of active side, and is recommended when the active side includes signi-

ficant tangential motion (as only the normal displacement is effectively transferred in this method).

use-virtual-polygon-approach

Uses new virtual polygon approach for interfaces.

Important

Note that case files created after ANSYS Fluent . will not show the virtual-polygon

option, since it is the default.

verbosity

Sets the mesh interface verbosity.

mesh-morpher-optimizer/

Enters the mesh morpher/optimizer menu in order to deform the mesh as part of a shape optimization

problem.This text command is only available when the define/enable-mesh-morpher-optimizer?

text command has been enabled.

deformation-settings/

Enters the deformation menu.This text command is only available if you have created a deformation

region using the define/mesh-morpher-optimizer/region/create or the define/mesh-

morpher-optimizer/region/define-bounding-box text command.

Displays a mesh check report in the console for the mesh displayed in the graphics window.The

mesh check report provides volume statistics, mesh topology and periodic boundary information,

verification of simplex counters, and verification of node position with reference to the  axis for

axisymmetric cases.This text command is only available if the define/mesh-morpher-optim-

izer/optimizer? text command is disabled.

deform-mesh

Modifies the mesh and updates the mesh display in the graphics window based on the parameter

and deformation settings.This text command is only available if the define/mesh-morpher-

optimizer/optimizer? text command is disabled.

motion-settings

Enters the motion settings menu, where you can create, modify, and delete the motions applied

to the control points.This text command is only available if the define/mesh-morpher-op-

timizer/set-control-point-distribution text command is set to unstructured.

create

Creates a new motion, by specifying the parameter, type of motion (translation, rotation, or

radial motion), directional settings, name, and control points. Note that for translations, the

values you enter for the direction components are multiplied with the value of the parameter

delete

Deletes an existing motion.

modify

Modifies the settings for an existing motion.

delete

modify

define/

read-from-file

Defines the settings for all the motions by reading an ASCII text file.

write-to-file

Writes the settings for all the motions to an ASCII text file.

read-motion-settings-from-file

Defines all of the motion settings by reading an ASCII text file.This text command is only available

if the define/mesh-morpher-optimizer/set-control-point-distribution text

command is set to regular.

reset-all-deformations

Undoes any deformations made to the mesh and updates the mesh display in the graphics window.

set-constraints

Defines the constraints on a boundary zone, in order to limit the freedom of a particular zone that

falls within the deformation region(s) during the morphing of the mesh.

set-constraints-multiple

Defines the constraints on multiple boundary zones, in order to limit the freedom of particular

set-parameters

Assigns translation direction components and a single parameter to a single control point in a region.

Note that the values you enter for the direction components are multiplied with the value of the

parameter to define the displacement applied to the control point.This text command is only

available if the define/mesh-morpher-optimizer/set-control-point-distribution

text command is set to regular.

set-parameters-multiple

Assigns translation direction components and multiple parameters to multiple control points in a

region. Note that the values you enter for the direction components are multiplied with the value

of the parameter to define the displacement applied to the control point.This text command is

only available if the define/mesh-morpher-optimizer/set-control-point-distri-

bution text command is set to regular.

write-motion-settings-to-file

Writes the motion settings to an ASCII text file.This text command is only available if the

define/mesh-morpher-optimizer/set-control-point-distribution text command

is set to regular.

morpher-summary

Displays a summary of the mesh morpher/optimizer settings in the console.This text command is only

available if you have created a deformation region using the define/mesh-morpher-optim-

izer/region/create or the define/mesh-morpher-optimizer/region/define-

bounding-box text command.

optimizer-parameters/

Enters the optimizer menu.This text command is only available when you have created a deformation

morpher-optimizer/region/define-bounding-box text command and have enabled the

define/mesh-morpher-optimizer/optimizer? text command.

convergence-criteria

Defines the convergence criteria for the optimizer.

custom-calculator

Enters the custom calculator menu, in order to define the objective function as a function of output

parameters.This menu is not available when the NEWUOA optimizer is selected using the

define/mesh-morpher-optimizer/optimizer-parameters/optimizer-type text

command.

define

Defines the custom objective function that will be minimized by the optimizer.

delete

Deletes the saved custom objective function.

command.

define

delete

example-obj-fn-definitions

Prints examples of custom objective function definitions in the console.

list-output-parameters

Prints a list of the output parameters that can be used to define the custom objective function.

disable-mesh-check

Specifies whether you want to disable the general mesh check that is part of the optimization

process.This check is conducted immediately after the mesh is deformed in every design stage,

and determines whether a solution is calculated. Disabling this check allows you to use mesh repair

commands (which can be set up using the define/mesh-morpher-optimizer/optimizer-

parameters/initial-commands text command) at the start of a design stage, so that an

accurate solution can be calculated.

end-commands

Specifies the commands (text commands or command macros) that will be executed after the

solution has run and converged for a design stage.This text command is not available when the

NEWUOA optimizer is selected using the define/mesh-morpher-optimizer/optimizer-

parameters/optimizer-type text command.

initial-commands

design has been modified, but before ANSYS Fluent has started to run the calculation for that

design stage.This text command is not available when the NEWUOA optimizer is selected using

the define/mesh-morpher-optimizer/optimizer-parameters/optimizer-type

initialization

Specifies how the solution variables should be treated after the mesh is deformed, that is, whether

they should be initialized to the values defined in the Solution Initialization task page, remain

the values obtained in the previous design iteration, or be read from a data file that you specify.

iterations-per-design

Defines the maximum number of iterations ANSYS Fluent will perform for each design change.

maximum-designs

Defines the maximum number of design stages the optimizer will undergo to reach the specified

define/

mesh-quality-check

Specifies if orthogonal quality should be used to determine whether a solution is calculated for a

mesh, and defines the minimum orthogonal quality value allowed (values may range from –,

where  represents the worst quality).

monitor/

Enters the monitor menu in order to plot and/or record optimization history data, that is, how the

value of the objective function varies with each design stage produced by the mesh morpher/op-

timizer.This text menu is not available when the NEWUOA optimizer is selected using the

command.

clear-opt-hist

Discards the optimization history data, including the associated files.

plot-hist

Displays an XY plot of the optimization history data generated during the last calculation. Note

that no plot will be displayed if the data was discarded using the define/mesh-morpher-

optimizer/optimizer-parameters/monitor/clear-optimization-monitor-

data text command.

plot?

Enables the plotting of the optimization history data in the graphics window.

write?

Enables the saving of the optimization history data to a file.

newuoa-initial-parameter-variation

plot?

write?

Defines how much the parameters will be allowed to vary during the initial calculations.This text

command is only available when the NEWUOA optimizer is selected using the define/mesh-

morpher-optimizer/optimizer-parameters/optimizer-type text command.

objective-function-definition

Specifies whether the format of the objective function is a user-defined function, a Scheme source

file, or a custom function based on output parameters.The custom function is defined using the

text commands in the define/mesh-morpher-optimizer/optimizer-parameters/cus-

tom-calculator menu.The objective-function-definition text command is not

available when the NEWUOA optimizer is selected using the define/mesh-morpher-optim-

izer/optimizer-parameters/optimizer-type text command.

optimize

Initiates the optimization process.This text command is only available if the define/mesh-

morpher-optimizer/optimizer? text command is enabled.

optimizer-type

Specifies which optimizer is to be used.You can select one of the six built-in optimizers (– and

), or specify that you will use Design Exploration in ANSYS Workbench (). Note that  is only

and Optimization in the User's Guide or Working With Input and Output Parameters in Workbench

in the ANSYS Fluent in Workbench User's Guide, respectively.

save-case-data-files

Sets up the automatic saving of intermediate case and data files during the optimization run, by

specifying: the frequency (in design iterations) with which file sets are saved; the maximum number

of file sets retained (after the maximum limit has been saved, the earliest file set will be overwritten

with the latest); and the root name assigned to the files (which will have the design iteration

number appended to it).

optimizer?

Enables the use of a built-in optimizer.This text command is only available if you have created a de-

formation region using the define/mesh-morpher-optimizer/region/create or the

define/mesh-morpher-optimizer/region/define-bounding-box text command.

parameter-settings/

Enters the parameters menu.

number-of-parameters

Defines the number of parameters that will be used to define the deformation.

parameter-bounds

Defines the minimum and maximum values allowed by the built-in optimizer for the parameters.

This text command is only available if the define/mesh-morpher-optimizer/optimizer?

text command is enabled.

parameter-value

Defines the value of a parameter.This value represents a magnitude that will then be used along

with other direction settings to define motions that produce an overall displacement for a given

control point.The value will specify a length in meters for translations and radial motions, and will

specify an angle in degrees for rotations; the units here will be used regardless of what units you

are using in the case. Note that you can enter a numeric value or define an input parameter (if you

have enabled the definition of input parameters using the define/parameters/enable-in-

TUI? text command).The parameter-value text command is only available in the following

situations:

if the define/mesh-morpher-optimizer/optimizer? text command is disabled

if the define/mesh-morpher-optimizer/optimizer? text command is enabled and

is selected for the optimizer type via the define/mesh-morpher-optimizer/optim-

izer-type text command

region/

Enters the region menu in order to define the regions of the domain where the mesh will be deformed

in order to optimize the shape.

control points

Enters the control points menu in order to create, modify, and/or delete control points.This text

command is only available if the define/mesh-morpher-optimizer/set-control-

point-distribution text command is set to unstructured.

create

Creates a new control point by defining the coordinates of a point within an existing deform-

ation region.

delete

Deletes existing control points.

define/

distribute-points-on-zone

Creates an approximate number of control points on the mesh nodes of a particular boundary

zone, with a distribution that is based on the distribution of the cell faces in that zone.

modify

Modifies the coordinates of existing control points.

Defines all of the control points by reading an ASCII text file.

Writes the control point coordinates to an ASCII text file.

create

Creates a new deformation region by specifying the name, number of control points (for a regular

distribution), dimensions, origin coordinates, the components of the direction vectors, and

create

whether to smooth the transitions of the mesh at the region boundaries (for an unstructured dis-

tribution).The region will be a “box”, that is, a rectangle for 2D cases or a rectangular hexahedron

for 3D cases. After you have created a deformation region, additional menus will be available in

the define/mesh-morpher-optimizer menu.

define-bounding-box

Creates a new deformation region by specifying the name, the bounding zones that best represent

the extents of the deformation region, the number of control points (for a regular distribution),

and whether to smooth the transitions of the mesh at the region boundaries (for an unstructured

distribution).The region will be a “box”, that is, a rectangle for 2D cases or a rectangular hexahedron

delete

Deletes a deformation region.

scaling-enlarge

Sets the scaling factor applied to the bounding box when you click the Enlarge button in the Re-

gions tab of the Mesh Morpher/Optimizer dialog box.

scaling-reduce

Sets the scaling factor applied to the bounding box when you click the Reduce button in the Re-

set-control-point-distribution

Specifies whether the control point distribution is regular (that is, spread in a regular distribution

throughout the entire deformation region) or unstructured (that is, distributed at specified locations).

mixing-planes/

Enters the mixing planes menu.

create

Creates a mixing plane.

delete

create

delete

Deletes a mixing plane.

list

Lists defined mixing plane(s).

set/

Sets global parameters relevant to mixing planes.

averaging-method

Sets the mixing plane profile averaging method.

Sets mixing plane under-relaxation factor.

fix-pressure-level

Sets fixed pressure level using value based on define/reference-pressure-location.

conserve-swirl/

Enters the menu to set swirl conservation in mixing plane menu.

enable?

Enables/disables swirl conservation in mixing plane.

verbosity?

Enables/disables verbosity in swirl conservation calculations.

report-swirl-integration

Reports swirl integration (Torque) on inflow and outflow zones.

conserve-total-enthalpy/

Enters the menu to set total enthalpy conservation in mixing plane menu.

enable?

Enables/disables total enthalpy conservation in mixing plane.

Enables/disables verbosity in total-enthalpy conservation calculations.

models/

Enters the models menu to configure the solver.

acoustics/

Enters the acoustics menu.

auto-prune

Enables/disables auto prune of the receiver signal(s) during read-and-compute.

broad-band-noise?

Enables/disables the broadband noise model.

convective-effects?

Enables/disables the convective effects option.

compute-write

Computes sound pressure.

define/

cylindrical-export?

Enables/disables the export of data in cylindrical coordinates.

display-flow-time?

Enables/disables the display of flow time during read-and-compute.

export-source-data-cgns?

Enables/disables the export of acoustic source data in CGNS format.

export-volumetric-sources?

Enables/disables the export of fluid zones.

export-volumetric-sources-cgns?

export-source-data?

Enables/disables the export of acoustic source data in ASD format during the wave equation

model run.

far-field-parameters/

Enters the menu to specify the far-field density and speed of sound. Note that this menu is currently

available only with the acoustics wave equation model.

far-field-density

Specifies the far-field density value for the acoustics wave equation model.

far-field-sound-speed

Specifies the far-field speed of sound value for the acoustics wave equation model.

ffowcs-williams?

Enables/disables the Ffowcs-Williams-and-Hawkings model.

moving-receiver?

Enables/disables the moving receiver option.

off?

Enables/disables the acoustics model.

read-compute-write

Reads acoustic source data files and computes sound pressure.

receivers

Sets acoustic receivers.

sources

Sets acoustic sources.

sources-fft/

Enters the acoustic sources fast Fourier transform (FFT) menu, to compute Fourier spectra from

acoustic source data (ASD) files, create postprocessing variables for the pressure signals, and write

CGNS files of the spectrum data.

read-asd-files

Reads ASD files to perform FFT of the pressure history field.

compute-fft-fields

Computes FFT of the read pressure histories.The computed spectra replace the pressure his-

tories in memory.

clean-up-storage-area

De-allocates memory used to store the pressure histories and their Fourier spectra, as well as

any created surface variables for the visualization.

write-cgns-files

Writes surface pressure spectra in CGNS format, which can be used for one-way coupling with

ANSYS Mechanical in the frequency domain.

fft-surface-variables/

Enters the menu to create surface variables from the computed Fourier spectra for visualization.

create-constant-width-bands

Selects up to  constant width bands and creates surface pressures level (SPL) variables

for them.

create-octave-bands

Creates surface pressure level (SPL) variables for  technical octaves.

create-third-bands

Creates surface pressure level (SPL) variables for  technical thirds.

create-set-of-modes

Selects up to  individual Fourier modes and create variable pairs for them, containing

the real and the imaginary parts of the complex Fourier amplitudes.

remove-variables

Removes all variables created in this menu.

wave-equation?

Enables/disables the wave equation model.

wave-equation-options/

Enters the menu to define the acoustics wave equation model options.

basic-shapes/

Enters the menu to define the geometry of the source mask and sponge layer using the basic

shapes, represented by the cell registers of the type "Region".

add-source-mask-shape

Adds a basic shape to the definition of the source mask geometry.

add-sponge-layer-shape

Adds a basic shape to the definition of the sponge layer geometry.

list-source-mask-shapes

List basic shapes, which are currently used in the definition of the source mask geometry.

list-sponge-layer-shapes

List basic shapes, which are currently used in the definition of the sponge layer geometry.

define/

list-region-registers

define/

List all available cell registers of the type "Region".

remove-source-mask-shape

Remove a basic shape from the definition of the source mask geometry.

remove-sponge-layer-shape

Remove a basic shape from the definition of the sponge layer geometry.

source-mask-udf

Specifies the name of a user-defined function, which defines geometry of the source mask.

sponge-layer-base-value

Specifies the base value of the artificial viscosity coefficient.

sponge-layer-factor

Specifies the factor of the artificial viscosity coefficient.

sponge-layer-udf

Specifies the name of a user-defined function, which defines geometry of the sponge layer.

time-filter-source?

Enables/disables a time filter for the sound source.

write-acoustic-signals

Writes on-the-fly sound pressure.

write-centroid-info

Writes centroid info.

addon-module

Loads addon module.

axisymmetric?

Specifies whether or not the domain is axisymmetric.

cht

Enters the cht (conjugate heat transfer) menu.

implicit-coupling?

Enables the implicit mapping scheme for any fluid-solid pair with a mapped mesh interface (only

required for cases set up in version . or earlier).

crevice-model?

Enables/disables the crevice model.

crevice-model-controls/

Enters the crevice model controls menu.

dpm/

Enters the dispersed phase model menu.

clear-particles-from-domain

Removes/keeps all particles currently in the domain.

collisions/

Enters the DEM collisions menu.

collision-mesh

Input for the collision mesh.

collision-pair-settings/

Supplies settings for collisions to a pair of collision partners.You will be prompted to specify

the Impact collision partner and the Target collision partner.

contact-force-normal

Sets the normal contact force law for this pair of collision partners.

contact-force-tangential

Sets the tangential contact force law for this pair of collision partners.

list-pair-settings

Lists the current settings for this pair of collision partners.

collision-partners/

Manages collision partners.

copy

Copies a collision partner.

create

Creates a collision partner.

delete

Deletes a collision partner.

list

Lists all known collision partners.

rename

Renames a collision partner.

dem-collisions?

Enables/disables the DEM collision model.

list-all-pair-settings

For each pair of collision partners, lists the collision laws and their parameters.

max-particle-velocity

Sets the maximum particle velocity that may arise from collisions.

erosion-dynamic-mesh/

Enters the menu to enable/configure/run the erosion-dynamic mesh interaction.

enable-erosion-dynamic-mesh-coupling?

Enables mesh deformation due to wall erosion.

general-parameters/

Enters the menu for setting erosion coupling with dynamic mesh.

define/

dynamic-mesh-settings

Sets parameters for dynamic mesh calculations.

erosion-settings

Sets parameters for erosion calculations.

participating-walls

Specifies all participating walls.

run-parameters/

Manages erosion-dynamic mesh run settings.

autosave-files

Sets the iteration increment and filename to save data files.

autosave-graphics

Sets the iteration increment to save graphics files.

flow-simulation-control

Sets the number of iterations per flow simulation step.

mesh-motion-time-step

Sets the mesh motion time stepping parameters and method.

simulation-termination

Sets the total time of erosion.

run-simulation

Performs a coupled erosion-dynamic mesh simulation.

create-injection

Creates an injection.

delete-injection

Deletes an injection.

injection-properties/

Enters the menu to set or display properties for one or more injections.

file/

Enters the menu to specify file injection settings.

filename

Specifies the name for the injection file.

repeat-interval-in-file

Puts the unsteady file injection into a time-periodic mode. For more information, see

User Input for File Injections in the Fluent User's Guide.

start-flow-time-in-file

Specifies the flow-time in the unsteady injection file from which ANSYS Fluent starts

reading the injection file. For more information, see User Input for File Injections in the

list/

Enters the menu to display the current properties for one or more injections.

list-picked-injections

Lists the injections that have been selected for display using pick-injections-

to-list.

list-picked-properties-to-list

Lists the properties that have been selected for display using pick-properties-

to-list.

list-property-values

Lists the settings for the properties selected with pick-properties-to-list.

This text command is only available when a single injection has been selected with

pick-injections-to-list.This option is available if at least two injections have

been selected.

list-uniform-values

Lists the settings for properties selected with pick-properties-to-list that

have uniform values for all of the injections selected with pick-injections-to-

list.This option is available if at least two injections have been selected.

list-values-per-injection

For each injection selected with pick-injections-to-list, lists the values for

properties selected with pick-properties-to-list.This option is available if at

least two injections ave been selected.

list-values-per-property

For each property selected with pick-properties-to-list, lists the values for

the injections selected with pick-injections-to-list.This option is available

if at least two injections have been selected.

pick-injections-to-list

Selects the injection or injections for which property values will be displayed.The use

of asterisks (*) as wildcards is supported.

pick-properties-to-list

Selects the property or properties for which values will be displayed.The use of asterisks

(*) as wildcards is supported.

set/

Enters the menu to set physical models such as drag and breakup for one or more injections.

Lists the injections selected for setting with pick-injections-to-set.

define/

location/

Enters the injection location settings menu.This command is only available when you

select the injection(s) using the prompts of the define/models/dpm/injec-

spatial-staggering/

Enters the injection spatial-staggering settings menu.

stagger-atomizer-positions?

Enables spatial staggering of the atomizer injection.This option is available

only if at least one atomizer injection has been selected using define/injec-

tions/properties/set/pick-injections-to-set.

stagger-radius

Specifies the stagger radius of the region from which particles are released.

This option is available only if at least one standard injection has been selected

using define/injections/properties/set/pick-injections-

to-set.

stagger-std-inj-positions?

Enables injection-specific spatial staggering of the particles.This option is

available only if at least one standard injection has been selected using

define/injections/properties/set/pick-injections-to-set.

physical-models

Enters the menu to set physical models such as drag and breakup for the selected in-

jections.This command is only available when you select the injection(s) using the

prompts of the define/models/dpm/injections/properties/set/pick-

injections-to-set text command.

brownian-motion

Enables Brownian motion effects for the currently selected injection(s).

drag-parameters

Sets the drag law and corresponding parameters for the currently selected injec-

tion(s).

particle-rotation

Enters the menu to set-up rotation related models.

enable-rotation

Enables/disables solution of ODE for the angular acceleration of particles.

magnus-lift-law

Sets the law for the rotational lift coefficient used in the formulation of Magnus

lift force.

rotational-drag-law

Sets the law for the rotational drag coefficient.

rough-wall-model

Enables/disables the rough wall model.

spray-secondary-breakup

Enters the menu for setting the breakup model and parameters for the currently

selected injection(s). Available commands are as those described under

define/models/dpm/spray-model/ with the addition of the following.

pick-injections-to-set

Selects the injection or injections for which properties will be set.The use of asterisks

list-particles

Lists particle streams in an injection.

modify-all-injections

Enters the menu to set properties for all injections.

injection-type

Defines injection type.

number-of-tries

Sets the number of stochastic tries.

random-eddy-lifetime?

Turns enable/disable a random eddy lifetime.

stochastic-tracking?

Turns enable/disable stochastic tracking.

time-scale-constant

Sets the time scale constant.

rename-injection

Renames an injection.

set-injection-properties

Sets injection properties.

Important

Drag and breakup model parameters for each injection are set instead in

/define/models/dpm/injections/injection-properties.

interaction/

Sets parameters for coupled discrete phase calculations.

coupled-calculations?

Selects whether or not to couple continuous and discrete phase calculations.

implicit-momentum-coupling?

Enables/disables implicit treatment for the DPM momentum source terms.

implicit-source-term-coupling?

Enables/disables implicit treatment for all DPM source terms.

define/

linear-growth-of-dpm-source-term?

Enables/disables the linear ramping up of the DPM source terms at every DPM iteration.

linearized-dpm-source-terms?

Enables/disables linearization of source terms for the discrete phase.

dpm-iteration-interval

Sets the frequency with which the particle trajectory calculations are introduced.

reset-sources-at-timestep?

Enables/disables flush of DPM source terms at beginning of every time step.

underrelaxation-factor

Sets the under-relaxation factor for the discrete phase sources.

update-dpm-sources-every-flow-iteration?

Enables/disables the update of DPM source terms every flow iteration (if this option is not en-

abled, the terms will be updated every DPM iteration).

numerics/

Enters the numerics menu to set numerical solution parameters.

automated-scheme-selection?

Enables/disables the adaptation of integration step length based on a maximum error.

average-DDPM-variables?

Enables/disables mesh node averaging of DDPM quantities.

average-each-step?

Enables/disables mesh node averaging during integration time step.

average-kernel

Specifies the averaging kernel to use for mesh node averaging.

average-source-terms?

Enables/disables mesh node averaging of DPM source terms.

coupled-heat-mass-update

Enables/disables coupled heat and mass update.

drag-law

Sets the drag law.

enable-node-based-averaging?

Enables/disables mesh node averaging of DPM quantities.

error-control?

Adapts integration step length based on a maximum error.

gaussian-factor

Specifies the Gaussian constant when using the gaussian kernel for mesh node averaging.

minimum-liquid-fraction

A droplet evaporates completely when the remaining mass is below this fraction of the initial

droplet mass.

tracking-parameters

Sets parameters for the (initial) tracking step length.

tracking-scheme

Specifies a tracking scheme.

underrelax-film-height

Sets the under-relaxation factor for the film height calculation.The recommended values range

between . (default) and ..

vaporization-limiting-factors

Sets the Vaporization Fractional Change Limits.

options/

Enters the options menu to set optional models.

allow-supercritical-pressure-vaporization?

Enforces the switching from vaporization to boiling even if the boiling point is not calculated

from the vapor pressure data. If the pressure in your model is above critical you must retain

the default setting (yes).This options is available only if when Pressure Dependent Boiling

is enabled in the Physical Models tab of the Discrete Phase Models dialog box. For more

details, see Enabling Pressure Dependent Boiling in the Fluent User's Guide.

Enables/disables Brownian motion of particles.

enable-contour-plots

Enables computation of mean and/or RMS values of additional discrete phase variables for

postprocessing.

ensemble-average

Ensembles average cloud properties.

erosion-accretion

Enables/disables erosion/accretion.

init-erosion-accretion-rate

Initializes the erosion/accretion rates with zero.

maximum-udf-species

Specifies the maximum number of species that will be accessible from discrete phase model

UDFs. Only species with indices up to this value are accessible in discrete phase model UDFs.

particle-radiation

Enables/disables particle radiation.

pressure-gradient-force

Enables/disables inclusion of pressure gradient effects in the particle force balance.

remove-wall-film-temperature-limiter?

Answering yes at the prompt removes the wall temperature limiter for Lagrangian wall-film

walls. If you enter no (default), two additional prompts will appear in the console allowing you

to define the temperature difference above the boiling point and to enable/disable the reporting

of the Leidenfrost temperature on the wall faces.

define/

scr-urea-deposition-risk-analysis/

Enters the menu for setting up the risk for solids deposit formation for the Selective Catalytic

Reduction (SCR) process. For more information, see Assessing the Risk for Solids Deposit

Formation During Selective Catalytic Reduction Process in the Fluent User's Guide.

cryst-depo-weight

Sets the weighting factor for crystallization reactions risk.

cryst-max-temp

Sets maximum temperature for urea crystallization.

cryst-min-mass-fract

Sets the minimum urea mass fraction for crystallization.

cryst-min-temp

Sets minimum temperature for urea crystallization.

enable?

Enables/disables the SCR urea deposition risk analysis.

heat-flux-based-risk-weight

Sets the weighting factor for heat flux-based component within hydrodynamic risk.

hydrodynamic-risk-weight

Sets the weighting factor for all hydrodynamic deposition risk.

seco-rx-max-temp

Sets maximum temperature for secondary reactions.

seco-rx-min-hnco

Sets the minimum HNCO mass fraction in the gas phase above the film for secondary reac-

tions.

seco-rx-min-temp

Sets minimum temperature for secondary reactions.

velocity-based-risk-weight

Sets the weighting factor for velocity-based component within hydrodynamic risk.

wall-face-zones

Lists the selected wall zones and allows you to modify the selection list.

stagger-spatially-atomizer-injections?

Enables/disables spatial staggering for atomizer and solid-cone injections.

stagger-spatially-standard-injections?

Enables/disables spatial staggering for standard (non-atomizer and non-solid-cone) injections.

Enables/disables temporal staggering.

Controls the percentage of every particle's initial time step that will be sampled.

saffman-lift-force

Enables/disables Saffman lift force.

Specifies the region over which to spatially stagger particles when particle-staggering is enabled

for non-atomizer injections.

step-report-sig-figures

Sets significant figures in the step-by-step report.

thermophoretic-force

Enables/disables thermophoretic force.

track-in-absolute-frame

Enables/disables tracking in absolute frame.

treat-multicomponent-saturation-temperature-failure?

Enables/disables dumping multicomponent particle mass into the continuous phase if the

two-way-coupling

Enables/disables calculation of DPM sources in TKE equation.

uniform-mass-distribution-for-injections?

Specifies a uniform distribution of mass over the cross-section of solid cone and atomizer in-

jections.This can become important when the mesh is smaller than the diameter (or another

characteristic size) of the injection.

use-absolute-pressure-for-vaporization?

Determines whether the absolute pressure or constant operating pressure (specified in

define/operating-conditions/operating-pressure) will be used in vaporization

rates calculations.

vaporization-heat-transfer-averaging

Enables averaging of the Spalding heat transfer term for the convection/diffusion-controlled

model.

vaporization-options

Sets Vaporization options.

virtual-mass-force

Enables/disables inclusion of the virtual mass force in the particle force balance.

parallel/

Enters the parallel menu to set parameters for parallel DPM calculations.

enable-workpile?

Turns on/off particle workpile algorithm.This option is only available when the

define/models/dpm/parallel/use-shared-memory option is selected.

expert/

Enters the menu for expert DPM parallel text commands.

define/

partition-method-hybrid-2domain

Enables/disables a partitioning method that is more granular and can yield faster calculations

(especially for cases that are running on a low to moderate number of processors).This

partitioning method is only applied when you use the DPM domain for the hybrid parallel

DPM tracking mode (that is, when you have enabled the define/models/dpm/paral-

lel/hybrid-2domain? text command).

hybrid-2domain?

Enables/disables the use of a second domain for DPM particle tracking.

n-threads

Sets the number of processors to use for DPM.This option is only available when the

define/models/dpm/parallel/enable-workpile? option is enabled.

report

Prints particle workpile statistics.This option is only available when the define/mod-

els/dpm/parallel/enable-workpile? option is enabled.

use-hybrid

report

Specifies that the calculations are performed using multicore cluster computing or shared-

memory machines.This option works in conjunction with openmpi for a dynamic load balancing

without migration of cells.

use-message-passing

Specifies that the calculations are performed using cluster computing or shared-memory ma-

chines.With this option, the compute node processes themselves perform the particle work

on their local partitions and particle migration to other compute nodes is implemented using

message passing primitives.

use-shared-memory

Specifies that the calculations are performed on shared-memory multiprocessor machines.

splash-options

Enters the splash option menu.

orourke-splash-fraction

Enables/disables the O’Rourke formulation (default for the Lagrangian Wall Film (LWF) model).

If the O’Rourke formulation is disabled, the Stanton formulation (default for the Eulerian Wall

Film (EWF) model) is used in a simulation.

splash-pdf-limiting

Sets the splash pdf limiting method. Available methods are: the splash pdf tail limiting (default

for the LWF model) and the splash pdf peak limiting (default for the EWF model). For the splash

pdf peak limiting, you will be prompted to specify the peak limiting value.

spray-model/

Enters the spray model menu.This command is available only if the breakup model enabled

globally.

breakup-model-summary

Current spray model settings.

consider-children-in-the-same-tracking-step?

Enables/disables collecting and tracking new generated child droplets within the same time

step.

droplet-coalescence?

step.

Enables/disables droplet coalescence when using the stochastic collision model.This option

is available if all injections have been selected and the DEM model is disabled.

droplet-collision?

Enables/disables droplet collision model.

enable-breakup?

Enables/disables breakup globally, but does not alter injection settings other than enable/dis-

able.

khrt-model

Sets the KHRT breakup model.

madabhushi-model

Sets the Madabhushi breakup model.

no-breakup

Disables the currently enabled breakup model.This option is available only if the breakup

model is enabled globally and for the selected injections, and not all injections have been se-

lected.

set-breakup

Enables/disables breakup model globally and uniformly specifies injection breakup parameters.

ssd-model

Sets the SSD breakup model.

tab-model

Sets the TAB breakup model.

tab-number-of-breakup-parcels

Sets the number of parcels to break up a droplet in the TAB model.

tab-randomize-breakup-parcel-diameter?

Enables sampling of diameter for each TAB breakup parcel from a Rosin-Rammler distribution

using a random number.

wave-allow-rayleigh-growth?

Allows treatment of the Rayleigh regime, in which a cylindrical liquid jet breaks into droplets

of larger diameter.This option is available only if the WAVE model is enabled.

wave-mass-cutoff

Sets the minimum percentage of parent parcel mass shed before new parcel creation.This

option is available only if the WAVE model is enabled.

wave-model

Sets the WAVE breakup model.

define/

wave-spray-angle-constant

define/

Sets the spray-angle constant to compute orthogonal velocity components of child droplets

after breakup.This option is available only if the WAVE model is enabled.

stripping-options

Enters the stripping options menu.

diameter-coefficient

Sets the diameter coefficient (  in Equation . in the Theory Guide)

mass-coefficient

Sets the mass coefficient (  in Equation . in the Theory Guide)

unsteady-tracking

Enables/disables unsteady particle tracking.

Sets DPM user-defined functions.

electric-potential?

Enables/disables the electric-potential model.

energy?

Enables/disables the energy model.

eulerian-wallfilm/

Enters the Eulerian wall film model menu.

enable-wallfilm-model?

Enables/disables Eulerian Wall Film Model.

initialize-wallfilm-model

Initializes Eulerian Wall Film Model.

solve-wallfilm-equation?

Activates Eulerian Wall Film Equations.

model-options

Sets Eulerian Wall Film Model Options.

film-material

Sets Film Material and Properties.

solution-options

Sets Eulerian Wall Film Model Solution Options.

frozen-flux?

Enables/disables frozen flux formulation for transient flows.

heat-exchanger/

Enters the heat exchanger menu.

dual-cell-model/

Enters the dual cell model menu.

add-heat-exchanger

Adds heat-exchanger.

alternative-formulation?

Enables/disables alternative formulation for heat transfer calculations.

delete-heat-exchanger

Deletes heat-exchanger.

heat-exchanger?

Enables/disables the dual cell heat-exchanger model.

modify-heat-exchanger

Modifies heat-exchanger.

plot-NTU

Plots NTU vs. primary mass flow rate for each auxiliary mass flow rate.

write-NTU

plot-NTU

write-NTU

Writes NTU vs. primary mass flow rate for each auxiliary mass flow rate.

macro-model/

Enters the heat macro-model menu.

delete-heat-exchanger-group

Deletes heat-exchanger group.

Enables/disables heat-exchanger model.

heat-exchanger-group

Defines heat-exchanger group.

heat-exchanger-macro-report

Reports the computed values of heat rejection, outlet temperature, and inlet temperature for

the macroscopic cells (macros) in a heat exchanger.

heat-exchanger-model

Defines heat-exchanger core model.

heat-exchanger-report

Reports the computed values of total heat rejection, outlet temperature, and inlet temperature

for a specified heat-exchanger core.

heat-exchanger-zone

Specifies the zone that represents the heat exchanger, the dimensions of the heat exchanger,

the macro grid, and the coolant direction and properties.

plot-NTU

write-NTU

define/

multiphase/

Enters the multiphase model menu.

body-force-formulation

Specifies body force formulation.

boiling-model-options

Specifies the boiling model options.You can choose the RPI boiling model, Non-equilib-

rium boiling, or Critical heat flux.

coupled-level-set

Enables coupled level set interface tracking method.

eulerian-parameters

Specifies Eulerian parameters.

expert-options

Specifies the volume fraction sub-time step calculation method and whether to solve vof every it-

eration.

interface-modeling-options

eration.

Specifies interface modeling options.

mixture-parameters

Specifies mixture parameters.

model

Specifies multiphase model.

number-of-phases

Specifies the number of phases.

vof-sub-models

Enables the Open Channel sub-model and/or the Open Channel Wave Boundary Condition sub-

model.

volume-fraction-parameters

Specifies volume fraction parameters.

wet-steam/

Enters the wet steam model menu.

compile-user-defined-wetsteam-functions

Compiles user-defined wet steam library.

enable?

Enables/disables the wet steam model.

load-unload-user-defined-wetsteam-library

Loads or unloads user-defined wet steam library.

set/

Enters the set menu for setting wet steam model options.

max-liquid-mass-fraction

Sets the maximum limit on the condensed liquid-phase mass-fraction to prevent divergence.

noniterative-time-advance?

Enables/disables noniterative time advancement scheme.

nox?

Enables/disables the NOx model.

nox-parameters/

Enters the NOx parameters menu.

inlet-diffusion?

Enables/disables inclusion of diffusion at inlets.

nox-chemistry

Selects NOx chemistry model.

nox-expert

Selects additional NOx equations.

nox-turbulence-interaction

Sets NOx turbulence interaction model.

population-balance/

Enters the population balance models menu.

model

Allows you to select the population balance model and set its parameters.

phenomena/

Enters the phenomena menu for population balance.

aggregation

Sets the aggregation kernel.

aggregation-factor

Specifies a factor that controls the intensity of the selected aggregation kernel.

breakage

Sets the breakage kernel.

breakage

breakage-factor

Specifies a factor that controls the intensity of the selected breakage kernel.

growth

Specifies the growth rate.

nucleation

Specifies the nucleation rate.

radiation/

Enters the radiation models menu.

define/

apply-full-solar-irradiation?

Enables/disables the application of the complete solar load to the first wavelength band only, re-

verting to the pre- R1 behavior of the Solar Load and Discrete Ordinates models.

blending-factor

Sets numeric option for Discrete Ordinate model. Make sure that Second Order Upwind is selected

for the Discrete Ordinates spatial discretization for the blending-factor option to appear in

the text command list.

discrete-ordinates?

Enables/disables discrete ordinates radiation model.

discrete-transfer?

Enables/disables discrete transfer radiation model.

do-acceleration?

Enables/disables the acceleration of the discrete ordinates (DO) radiation model calculations. Note

that this text command is only available when running on Linux in parallel.

do-coupling?

Enables/disables DO/energy coupling.

solar-irradiation?

Enables/disables the solar irradiation model.

dtrm-parameters/

Enters the dtrm parameters menu.

check-ray-file

Reads DTRM rays file.

controls

Sets dtrm solution controls.

make-globs

Makes globs (coarser mesh) for radiation.

ray-trace

Creates DTRM rays for radiation.

fast-second-order-discrete-ordinate?

Enables/disables the fast-second-order option for Discrete Ordinate Model.

mc-model-parameters

Specifies Monte Carlo model parameters.This text command is available only when the Monte

Carlo model is enabled.

mc-under-relaxation

Sets the under-relaxation factor for Monte Carlo radiation sources used in the energy equation.

method-partially-specular-wall

Sets the method for partially specular wall with discrete ordinate model.

montecarlo?

Enables/disables the Monte Carlo radiation model.

non-gray-model-parameters

Sets parameters for non-gray model.

p1?

Enables/disables P1 radiation model.

radiation-iteration-parameters

Sets iteration parameters for radiation models.

radiation-model-parameters

Sets parameters for radiation models.

rosseland?

Enables/disables Rosseland radiation model.

s2s?

Enables/disables S2S radiation model.

s2s-parameters/

Enters the S2S parameters menu.

compute-fpsc-values

Computes only fpsc values based on current settings

compute-vf-only

Computes/writes view factors only.

compute-write-vf

Computes/writes surface clusters and view factors for S2S radiation model.

non-participating-boundary-zones-temperature

Sets temperature for the non-participating boundary zones.

print-thread-clusters

Prints the following for all boundary threads: thread-id, number of faces, faces per surface

cluster, and the number of surface clusters.

print-zonewise-radiation

Prints the zonewise incoming radiation, viewfactors, and average temperature.

read-vf-file

Reads S2S file.

set-global-faces-per-surface-cluster

Sets global value of faces per surface cluster for all boundary zones.

set-vf-parameters

Sets the parameters needed for the viewfactor calculations.

split-angle

Sets split angle for the clustering algorithm.

use-new-cluster-algorithm

Uses the new surface clustering algorithm.

define/

use-old-cluster-algorithm

Uses the old surface clustering algorithm.

solar?

Enables/disables solar model.

solar-calculator

Calculates sun direction and intensity.

solar-parameters/

Enters the solar parameters menu.

autoread-solar-data

Sets autoread solar data parameters.

autosave-solar-data

Sets autosave solar data parameters.

ground-reflectivity

Sets ground reflectivity parameters.

illumination-parameters

Sets illumination parameters.

iteration-parameters

Sets update parameters.

quad-tree-parameters

Sets quad-tree refinement parameters.

scattering-fraction

Sets scattering fraction parameters.

solar-thread-control

Sets the number of threads to run the solar flux calculation.This item appears only when running

in parallel with nodes located on a separate machine from the one running the host process

and Solar Ray Tracing is enabled.

sol-adjacent-fluidcells

Sets solar load on for adjacent fluid cells.

sol-camera-pos

Sets camera position based on sun direction vector.

sol-on-demand

Sets solar load on demand.

sun-direction-vector

Sets sun direction vector.

use-direction-from-sol-calc

Sets direction computed from solar calculator.

solution-method-for-do-coupling

Enables/disables the solution method for DO/energy coupling.

target-cells-per-volume-cluster

Sets the amount of coarsening of the radiation mesh for the Monte Carlo radiation model. A

number greater than one implies coarsening, whereas equal to one implies no coarsening.

wsggm-cell-based

Enables/disables WSGGM cell based method. Note that when enabled, the wsggm-cell-based

option will become available in the Absorption Coefficient drop-down list in the Create/Edit

shell-conduction/

Enters the shell conduction models menu.

enhanced-encapsulation?

Enables/disables an enhanced routine for the encapsulation of coupled walls during mesh parti-

tioning that is enabled by default when shell conduction and/or the surface to surface (S2S) radiation

model is used.

multi-layer-shell?

Enables/disables the ability to define multi-layer shell conduction for walls. Note that the warped-

face gradient correction (WFGC) is not supported when multi-layer shells are disabled.

read-csv

Defines the shell conduction settings by reading a CSV file.

save-shell-zones?

Enables the saving of shell zones to case files.

settings

Enables shell conduction and defines the settings for any wall or group of walls by manually entering

the number and properties of the layers.

write-csv

Writes your saved shell conduction settings to a CSV file.

solidification-melting?

Enables/disables the solidification and melting model.

solver/

Enters the menu to select the solver.

density-based-explicit

Enables/disables the density-based-explicit solver.

density-based-implicit

Enables/disables the density-based-implicit solver.

Enables/disables the pressure-based solver.

soot?

Enables/disables the soot model.

soot-parameters/

Enters the soot parameters menu.

define/

soot?

define/

modify-schmidt-number?

Changes the turbulent Schmidt number for soot/nuclei equations.

soot-model-parameters

Selects soot model parameters.

soot-process-parameters

Selects soot process parameters.

soot-radiation-interaction

Enables/disables the soot-radiation interaction model.

soot-turbulence-interaction

Sets soot-turbulence interaction model.

sox?

Enables/disables the SOx model.

sox-parameters/

Enters the SOx parameters menu.

s-atom-balance?

Enables/disables S-atom mass balance calculation.

sox-chemistry

Selects the SOx chemistry model.

sox-turbulence-interaction

Sets the SOx /turbulence interaction model.

species/

Enters the species models menu.

CHEMKIN-CFD?

Enables/disables the ANSYS CHEMKIN-CFD solver.

CHEMKIN-CFD-parameters/

Enters the expert CHEMKIN-CFD parameters menu.

add-cell-monitor

Monitors cell for debug output.

advanced-options

Sets advanced parameter options.

basic-options

Sets basic parameter options.

delete-cell-monitors

Deletes cell monitors.

list-cell-monitors

Lists cell monitors.

clear-isat-table

Clears ISAT table.

coal-calculator

Sets up coal modeling inputs.

decoupled-detailed-chemistry?

Enables/disables the Decoupled Detailed Chemistry model.

diffusion-energy-source?

Enables/disables diffusion energy source.

electro-chemical-surface-reactions?

Enables/disables electrochemical surface reactions.

epdf-energy?

Enables/disables EPDF energy option.

flamelet-expert

Sets flamelet expert parameters.

full-tabulation?

Enables/disables building of a full -mixture fraction table

heat-of-surface-reactions?

Enables/disables heat of surface reactions.

ignition-model?

Enables/disables the ignition model.

ignition-model-controls

Sets ignition model parameters.

import-flamelet-for-restart

Imports Flamelet File for Restart.

inert-transport-controls

Sets inert transport model parameters.

inert-transport-model?

Enables/disables the inert transport model.

integration-parameters

Sets chemistry ODE integrator parameters. Enables/disables stiff chemistry acceleration methods

and set their parameters.

define/

init-unsteady-flamelet-prob

Initializes Unsteady Flamelet Probability.

liquid-energy-diffusion?

Enables/disables energy diffusion for liquid regime.

liquid-micro-mixing?

Enables/disables liquid micro mixing.

mass-deposition-source?

Enables/disables mass deposition source due to surface reactions.

mixing-model

Sets PDF Transport mixing model.

multicomponent-diffusion?

Enables/disables multicomponent diffusion.

non-premixed-combustion?

Enables/disables non-premixed combustion model.

non-premixed-combustion-expert

Sets PDF expert parameters.

non-premixed-combustion-parameters

Sets PDF parameters.

off?

Enables/disables solution of species models.

partially-premixed-combustion?

Enables/disables partially premixed combustion model.

partially-premixed-combustion-expert

partially-premixed-combustion-parameters

partially-premixed-properties

Sets/changes partially-premixed mixture properties.This command is only available when par-

tially-premixed-combustion? is enabled.

re-cacl-par-premix-props

Re-calculates partially-premixed properties.This command is only available when partially-

premixed-combustion? is enabled.

particle-surface-reactions?

Enables/disables particle surface reactions.

pdf-transport?

Enables/disables the composition PDF transport combustion model.

pdf-transport-expert?

Enables/disables PDF Transport expert user.

premixed-model

Sets premixed combustion model.

premixed-combustion?

Enables/disables premixed combustion model.

reaction-diffusion-balance?

Enables/disables reaction diffusion balance at reacting surface for surface reactions.

reacting-channel-model?

Enables/disables the Reacting Channel Model.

reacting-channel-model-options

Sets Reacting Channel Model parameters.

reactor-network-model?

Enables/disables the Reactor Network Model.

relax-to-equil?

Enables/disables the Relaxation to Chemical Equilibrium model.

save-gradients?

Enables/disables storage of species mass fraction gradients.

set-premixed-combustion

Sets premixed combustion parameters.

set-turb-chem-interaction

Sets EDC model constants.

spark-model

Switches between the R15 and R14. spark models and sets spark model parameters.

species-migration?

Includes species migration in electric field.This command is available only when the electrochem-

ical surface reactions are enabled.

species-transport-expert

Sets the convergence acceleration expert parameters.This command is only available when the

species transport model is enabled.

use convergence acceleration method?

Answering yes at the prompt, uses a combination of different convergence acceleration

techniques. If you enter no (default), additional options will be displayed in the console.

Use species clipping?

Enables/disables the explicit clipping of species between  and .

Linearize higher order convection sources?

Enables/disables linearization of higher order convection sources.

Linearize secondary diffusion sources?

Enables/disables linearization of species secondary diffusion sources.

define/

Enable mesh quality based first-second order species blending?

Enables/disables skewness-based blending of first and second order convection.

Minimum cell quality threshold for blending

Specifies the minimum cell orthogonal quality for blending.

species-transport?

Enables/disables the species transport model.

stiff-chemistry?

Enables/disables stiff chemistry option.

surf-reaction-aggressiveness-factor?

Sets the surface reaction aggressiveness factor.

surf-reaction-netm-params

Sets the surface reaction parameters for the Non-Equilibrium Thermal Model.

thermal-diffusion?

Enables/disables thermal diffusion.

thickened-flame-model?

Enables/disables the Relaxation to Chemical Equilibrium model

volumetric-reactions?

Enables/disables volumetric reactions.

wall-surface-reactions?

Enables/disables wall surface reactions.

steady?

Enables/disables the steady solution model.

structure

Enters the structure model menu.

controls

Enters the structure controls menu.

steady?

structure

controls

Sets the algebraic multigrid (AMG) stabilization method for the structural model calculations.

max-iter

Sets the maximum number of iterations for the structural model calculations.

numerical-damping-factor?

Sets the damping factor for the structural model (that is, the amplitude decay factor  in

expert

Enters the structure expert menu.

explicit-fsi-force?

Enables/disables an explicit fluid-structure interaction force.

include-pop-in-fsi-force?

Enables/disables the inclusion of operating pressure into the fluid-structure interaction force.

include-viscous-fsi-force?

Enables/disables the inclusion of a viscous fluid-structure interaction force.

linear-elasticity?

Enables the linear elasticity model.

structure-off?

Disables the structural model.

swirl?

Enables/disables axisymmetric swirl velocity.

unsteady-1st-order?

Selects the first-order implicit formulation for transient simulations.

unsteady-2nd-order-bounded?

Selects the bounded second-order implicit formulation for transient simulations.

unsteady-2nd-order?

Selects the second-order implicit formulation for transient simulations.

unsteady-global-time?

Selects the explicit transient formulation.This text command is only available for unsteady cases that

use the density-based solver with the explicit formulation.

unsteady-structure-euler?

Selects the backward Euler method for the direct time integration of the finite element semi-discrete

equation of motion.This text command is only available for transient simulations that use the structural

model.

unsteady-structure-newmark?

model.

Selects the Newmark method for the direct time integration of the finite element semi-discrete equation

of motion.This text command is only available for transient simulations that use the structural model.

viscous/

Enters the viscous model menu.

add-intermittency-transition-model?

Enables/disables the Intermittency Transition model to account for transitional effects.This text

command is only available for the BSL -

, SST -

, Scale-Adaptive Simulation with BSL / SST,

and Detached Eddy Simulation with BSL / SST models.

buoyancy-effects?

Enables/disables effects of buoyancy on turbulence.

curvature-correction-ccurv

Sets the strength of the curvature correction term.The default value is .This is available after the

curvature-correction? option is enabled.

.

define/

curvature-correction?

Enables/disables the curvature correction.

des-limiter-option

Selects the DES limiter option (none, F1, F2, Delayed DES, or Improved Delayed DES).

geko-options/

Enters the GEKO model menu..

csep

Sets csep, the parameter to optimize flow separation from smooth surfaces.

cnw

Sets cnw, the parameter to optimize flow in non-equilibrium near wall regions.

cmix

Sets cmix, the parameter to optimize strength of mixing in free shear flows.

cjet

Sets cjet, the parameter to optimize free shear layer mixing (optimize free jets independent

of mixing layer).

blending-function

Sets the blending function, which deactivates cmix and cjet inside boundary layers.

creal

Sets creal, a realizability limiter that ensures positive normal stresses in the entire domain.

cnw_sub

creal

cnw_sub

Sets cnw_sub, which allows the adjustment of log-layer and cf.

cjet_aux

Sets cjet_aux, which allows fine-tuning of the parameter to optimize free jets.

cbf_tur

Sets cbf_tur, a factor for the main blending factor, controlling the thickness of the layer near

walls.

cbf_lam

Sets cbf_lam, a part of the blending function and shields the laminar boundary layer.

geko-defaults

Restores the defaults of all GEKO parameters.

wall-distance-free?

Enables/disables the wall distance free version of the GEKO model.

detached-eddy-simulation?

Enables/disables detached eddy simulation.

inviscid?

Enables/disables inviscid flow model.

ke-easm?

Enables/disables the EASM -  turbulence model.

ke-realizable?

Enables/disables the realizable -  turbulence model.

ke-rng?

Enables/disables the RNG -  turbulence model.

ke-standard?

Enables/disables the standard -  turbulence model.

k-kl-w?

Enables/disables the k-kl-

kw-easm?

Enables/disables the EASM -

kw-low-re-correction?

Enables/disables the -

low Re option.

kw-shear-correction?

shear-flow correction option.This text command is only available for the

standard -

kw-bsl?

Enables/disables the baseline (BSL) -

kw-geko?

Enables/disables the generalized -

(GEKO) turbulence model.

kw-sst?

Enables/disables the SST -

kw-standard?

Enables/disables the standard -

laminar?

Enables/disables laminar flow model.

large-eddy-simulation?

kw-sst?

laminar?

Enables/disables large eddy simulation.

les-dynamic-energy-flux?

Enables/disables the dynamic sub-grid scale turbulent Prandtl Number.

les-dynamic-scalar-flux?

Enables/disables the dynamic sub-grid scale turbulent Schmidt Number.

les-subgrid-dynamic-fvar?

Enables/disables the dynamic subgrid-scale mixture fraction variance model.

les-subgrid-smagorinsky?

Enables/disables the Smagorinsky-Lilly subgrid-scale model.

les-subgrid-tke?

Enables/disables kinetic energy transport subgrid-scale model.

define/

les-subgrid-wale?

Enables/disables WALE subgrid-scale model.

les-subgrid-wmles-s_minus_omega?

Enables/disables the WMLES -  subgrid-scale model.

les-subgrid-wmles?

Enables/disables the WMLES subgrid-scale model.

mixing-length?

Enables/disables mixing-length (algebraic) turbulence model.

multiphase-turbulence/

Enters the multiphase turbulence menu.

multiphase-options

Enables/disables multiphase options.

rsm-multiphase-models

Selects Reynolds Stress multiphase model.

turbulence-multiphase-models

Selects -  multiphase model.

near-wall-treatment/

Enters the near wall treatment menu.

enhanced-wall-treatment?

Enables/disables enhanced wall functions.

menter-lechner?

Enables/disables the Menter-Lechner near-wall treatment.

non-equilibrium-wall-fn?

Enables/disables non-equilibrium wall functions.

scalable-wall-functions?

Enables/disables scalable wall functions.

standard-wall-fn?

Enables/disables standard wall functions.

user-defined-wall-functions?

Enables/disables user-defined wall functions.

werner-wengle-wall-fn?

Enables/disables Werner-Wengle wall functions.

wf-pressure-gradient-effects?

Enables/disables wall function pressure- gradient effects.

wf-thermal-effects?

Enables/disables wall function thermal effects.

reynolds-stress-model?

Enables/disables the Reynolds-stress turbulence model.

rng-differential-visc?

Enables/disables the differential-viscosity model.

rng-swirl-model?

Enables/disables swirl corrections for rng-model.

rsm-bsl-based?

Enables/disables the stress-BSL Reynolds stress model.

rsm-linear-pressure-strain?

Enables/disables the linear pressure-strain model in RSM.

rsm-omega-based?

Enables/disables the stress-omega Reynolds stress model.

rsm-or-earsm-geko-option?

Enables/disables the RSM or EARSM versions of the GEKO model.

rsm-solve-tke?

Enables/disables the solution of T.K.E. in RSM model.

rsm-ssg-pressure-strain?

Enables/disables quadratic pressure-strain model in RSM.

rsm-wall-echo?

Enables/disables wall-echo effects in RSM model.

sa-alternate-prod?

Enables/disables strain/vorticity production in Spalart-Allmaras model.

sa-damping?

Enables/disables full low-Reynolds number form of Spalart-Allmaras model.

Note

This option is only available if your response was no to sa-enhanced-wall-

treatment?.

sa-enhanced-wall-treatment?

Enables/disables the enhanced wall treatment for the Spalart-Allmaras model. If disabled, no

smooth blending between the viscous sublayer and the log-law formulation is employed, as was

done in versions previous to Fluent .

sas?

Enables/disables Scale-Adaptive Simulation (SAS) in combination with the SST -

model.

sas?

model.

spalart-allmaras?

Enables/disables Spalart-Allmaras turbulence model.

define/

transition-sst?

Enables/disables the transition SST turbulence model.

trans-sst-roughness-correlation?

Enables/disables the Transition-SST roughness correlation option.

turb-compressibility?

Enables/disables the compressibility correction option.

turbulence-expert/

Enters the turbulence expert menu.

kato-launder-model?

Enables/disables Kato-Launder modification.

kw-add-des?

Enables/disables Detached Eddy Simulation (DES) in combination with the currently selected

BSL -

model or transition SST model.This text command is only available for transient cases.

kw-add-sas?

Enables/disables Scale-Adaptive Simulation (SAS) in combination with the currently selected

based URANS turbulence model.This text command is only available for transient cases.

kw-vorticity-based-production?

Enables/disables vorticity-based production.

low-re-ke?

Enables/disables the low-Re -  turbulence model.

low-re-ke-index

Specifies which low-Reynolds-number -  model is to be used. Six models are available:

Model

Index

Abid

Lam-Bremhorst

Launder-Sharma

Yang-Shih

Abe-Kondoh-Nagano

Chang-Hsieh-Chen

Contact your ANSYS, Inc. technical support engineer for more details.

production-limiter?

Enables/disables Production Limiter modification.

non-newtonian-modification?

Enables/disables non-Newtonian modification for Lam-Bremhorst model.

restore-sst-v61?

Enables/disables SST formulation of v6..

rke-cmu-rotation-term?

Modifies the

definition for the realizable -  model.

Important

Important

Note that the use of the realizable -  model with multiple reference frames

is not recommended. This text command is provided for expert users who

want to experiment with this combination of models. Others should use it

only on the advice of a technical support engineer.

sbes-sdes-hybrid-model

Selects the hybrid model, to specify whether you want to apply the Shielded Detached Eddy

Simulation (SDES) model, Stress-Blended Eddy Simulation (SBES), or SBES with a user-defined

function.

sbes-sgs-option

Selects the subgrid-scale model for the LES portion of your Stress-Blended Eddy Simulation

(SBES).

sbes-update-interval-k-omega

Sets the number of time steps between updates of the k-ω part of the SBES model.

thermal-p-function?

Enables/disables Jayatilleke P function.

turb-add-sbes-sdes?

Enables/disables the Stress-Blended Eddy Simulation (SBES) model or Shielded Detached Eddy

Simulation (SDES) model.

turb-non-newtonian?

Enables/disables turbulence for non-Newtonian fluids.

turbulence-damping?

Enables/disables turbulence damping and sets turbulence damping parameters.

turb-pk-compressible?

Enables/disables turbulent production due to compressible divergence.

Selects user-defined functions to define the turbulent viscosity and the turbulent Prandtl and

Schmidt numbers.

user-defined-transition

Sets user-defined transition correlations.

v2f?

Enables/disables V2F turbulence model.

zero-equation-hvac?

Enables/disables zero-equation HVAC turbulence model.

named-expressions/

Enters the named expressions menu.

define/

add/

Creates a new named expression.

delete/

define/

add/

delete/

Allows you to delete a named expression, as long as it is not in use.

edit/

Allows you to edit the definition of a named expression.

list/

Lists all of the currently defined named expressions.

list-properties/

Lists the definition of a named expression.

operating-conditions/

Enters the define operating conditions menu.

gravity

Sets gravitational acceleration.

gravity-mrf-rotation

Enables/disables rotation of gravity vector in moving reference frame simulations. If enabled, the

gravity vector will rotate with respect to the moving reference frame such that the direction of gravity

in global coordinates remains fixed.

operating-density?

Enables/disables use of a specified operating density.

operating-pressure

Sets the operating pressure.

operating-temperature

Sets the operating temperature for Boussinesq.

reference-pressure-location

Sets the location of the cell whose pressure value is used to adjust the gauge pressure field for incom-

pressible flows that do not involve any pressure boundaries.

set-state

Selects state for real gas EOS subcritical condition.

used-ref-pressure-location

See the actual coordinates of the reference pressure used.

use-inlet-temperature-for-operating-density

Uses inlet temperature to calculate operating density.

overset-interfaces/

Enters the overset interfaces menu.

check

Checks the integrity of the overset interfaces. Reports orphan cells and errors in the domain connectivity.

clear

Clears the domain connectivity of an overset interface.This text command is only available when

clear

define/overset-interfaces/options/expert is set to yes.

clear-all

Clears the domain connectivity of all overset interfaces.This text command is only available when

create

Creates an overset interface.

cut-control/

Enters the overset hole cut control menu.

add

Adds a hole cut control, so that a boundary zone does not cut specified cell zones.

cut-seeds/

Enters the overset hole cut seeds menu.

cut-seeds-for-all-component-zones?

Specifies whether all component zones get cut seeds, which cut pilot holes into the overlapping

meshes that will then be enlarged during overlap minimization.

delete

Deletes the hole cut control for a boundary zone.

Deletes the hole cut controls for all boundary zones.

list

Lists the defined hole cut controls.

debug-hole-cut

Debugging tool to troubleshoot hole cutting of overset interfaces.This text command is only available

when define/overset-interfaces/options/expert is set to yes.

delete

Deletes an overset interface.

Deletes all overset interfaces in the domain.

display-cells

Displays the overset cells marked using the text command define/overset-interfaces/mark-

cells.

grid-priorities

Allows you to specify grid priorities on background and component meshes, used in the overlap min-

imization of an overset interface.

intersect

Executes the hole cutting of an overset interface and establishes the domain connectivity.This text

command is only available when define/overset-interfaces/options/expert is set to

yes.

define/

intersect-all

yes.

define/

Executes hole cutting for all overset interfaces in the domain.This text command is only available

list

Lists information about the overset interfaces.The output depends on the overset verbosity setting.

mark-cell-change

Marks cells that have undergone a specified overset cell type change (from solve, receptor, or

dead to any other type) in the last time step. Adaption registers are automatically filled based on these

markings.This text command is only available for unsteady simulations and if define/overset-

interfaces/options/expert is set to yes.

mark-cells

Marks the specified overset cells (solve, receptor, donor, orphan, or dead) and fills registers based on

the markings. Display the marked cells via the text command define/overset-interfaces/dis-

play-cells.

options/

Enters the overset interface options menu.

auto-create?

Enables the automatic creation of a default overset interface during initialization or mesh motion

update.

donor-priority-method

Allows you to specify whether the cell donor priority used in the overlap minimization of an overset

interface is inversely proportional to either the cell size or the distance to the nearest boundary.

expert

Enables / disables overset-related expert tools.

extended-donor-search?

Enables / disables modified donor search parameters.When enabled, more conservative overset

parameters are used for the creation of the overset interface (at the cost of increased processing

time).This text command is only available when define/overset-interfaces/options/ex-

pert is set to yes.

minimize-overlap?

Allows you to disable overlap minimization during hole cutting.

node-connected-donors?

Allows you to switch between face or node connected donor cells.This text command is only

available when define/overset-interfaces/options/expert is set to yes.

overlap-boundaries?

Allows you to disable the detection of overlapping boundaries during hole cutting, in order to reduce

the computational expense for cases that do not include such boundaries.When enabled, this text

command also allows you to specify which boundary zones should be considered when detecting

overlapping boundaries; this can be helpful when the default hole cutting process fails.

render-receptor-cells?

Allows you to enable visualization of receptor cells in contour and mesh displays.

solve-island-removal

Sets the method used to control the removal of isolated patches of solve cells.This text command

is only available when define/overset-interfaces/options/expert is set to yes.

transient-caching

Sets the options to control caching of entities in transient overset simulations.This text command

update-before-case-write?

Enables/disables the updating of the overset interfaces before writing a case file in the hierarchical

data format (HDF).This text command is only available when define/overset-interfaces/op-

tions/expert is set to yes.

verbosity

Specifies the level of detail printed in the console about overset interfaces.

parameters/

enable-in-TUI?

Enables/disables parameters in the text user interface.

input-parameters/

Enters the input-parameters menu.

delete

Deletes an input parameter.

edit

Edits an input parameter.

output-parameters/

Enters the output-parameters menu.

create

Creates an output parameter.

delete

Deletes an output parameter.

edit

Edits an output parameter.

print-all-to-console

Displays all parameter values in the console.

print-to-console

Displays parameter value in the console.

rename

Renames an output parameter.

write-all-to-file

Writes all parameter values to file.

define/

Writes parameter value to file.

periodic-conditions/

Enters the periodic conditions menu.

massflow-rate-specification?

Enables/disables specification of mass flow rate at the periodic boundary.

pressure-gradient-specification?

Enables/disables specification of pressure gradient at the periodic boundary.

phases/

Enters the phases menu.

iac-expert/

Enters the IAC expert setting menu.

hibiki-ishii-model

Sets Hibiki-Ishii model coefficients.

ishii-kim-model

Sets Ishii-Kim model coefficients.

yao-morel-model

Sets Yao-Morel model coefficients.

interaction-domain

Sets models and properties for a domain of this type.

phase-domain

set-domain-properties/

Enters the menu to set phase domain properties.

change-phases-names?

Allows you to change the names of all the phases in your simulation.

interaction-domain/

Enters the menu to set the interaction domain properties.

forces/

Enters the menu to set interfacial forces models.

drag

Specifies the drag function, drag modification, and drag factor for each pair of phases.This

forces/

drag

command is available only with the Eulerian and Mixture multiphase models.

lift

Specifies the lift function for each pair of phases.This command is available only with the

restitution

Specifies the restitution coefficient for collisions between each pair of granular phases, and

for collisions between particles of the same granular phase.This command is available only

for multiphase flows with two or more granular phases.

slip-velocity

Specifies the slip velocity function for each secondary phase with respect to the primary

phase.This command is available only for the Mixture multiphase model.

surface-tension/

Enters the menu to set surface tension models

jump-adhesion?

Enables/disables the treatment of the contact angle specification at the porous jump

boundary.This command is available only for the VOF multiphase model with the

continuum surface stress model option and when sfc-modeling? is enabled.

sfc-modeling?

Allows you to include the effects of surface tension along the fluid-fluid interface.This

option is only available for the VOF and Eulerian multiphase models.

sfc-model-type

Selects the surface tension model.You can choose between the continuum surface

force and continuum surface stress methods.This item is available only when sfc-

modeling? is enabled.

sfc-tension-coeff

Specifies the surface tension coefficient for each pair of phases.

wall-adhesion?

Enables/disables the specification for a wall adhesion angle.This item is available only

when sfc-modeling? is enabled.

turbulent-dispersion

Specifies the turbulent dispersion model for each primary-secondary phase pair.This

command is available only with the Eulerian multiphase model.

turbulence-interaction

Specifies the turbulence interaction model for each primary-secondary phase pair.This

virtual-mass/

Enters the menu to set virtual mass models.

virtual-mass?

Allows you to include the virtual mass force effect that occurs when a secondary phase

accelerates relative to the primary phase.This command is available only with the Eu-

lerian multiphase model.

vmass-coeff

Specifies the virtual mass coefficient for each pair of phases.This option is available

only if virtual-mass? is enabled.

define/

vmass-implicit?

Enables/disables the implicit method for the virtual mass force.This option can improve

convergence in some cases.This option is available only if virtual-mass? is enabled.

vmass-implicit-options

Specifies what form of the implicit method to use (default, option-, or option-

). default models the entire virtual mass force while option- and option-

model truncated expressions which may further improve convergence.This option is

available only if vmass-implicit? is enabled.

wall-lubrication

Specifies the wall lubrication model for each primary-secondary phase pair.This command

is available only with the Eulerian multiphase model.

heat-mass-reactions/

Enters the menu to set heat, mass-transfer, and reaction models.

cavitation/

Enters the menu to set cavitation models.This option is available only for the Mixture

multiphase model with the Singhal-et-al cavitation model enabled via solve/set/ex-

pert.

cavitation?

Allows you to include the effects of cavitation.When the cavitation is enabled, you

must specify vaporization pressure, surface tension coefficient, and non-condensable

gas mass fraction using the define/phases/set-domain-properties/inter-

action-domain/heat-mass-reactions/cavitation/caviation text

command. If multiple species are included in one or more secondary phases, or the

heat transfer due to phase change is considered, the mass transfer mechanism must

be defined before enabling the cavitation model.

Sets the vaporization pressure, surface tension coefficient, and non-condensable gas

mass fraction.This command is available only when cavitation? is enabled.

heat-coeff

Species the heat transfer coefficient function between each pair of phases (constant-

htc, nusselt-number, ranz-marshall, hughmark, tomiyama, fixed-to-sat-

temp, two-resistance, or user-defined).This command is enable only with the

mass-transfer

Sets the mass transfer mechanisms.

reactions

Allows you to define multiple heterogeneous reactions and stoichiometry.This option is

available only with the species model.

interfacial-area/

Enters the menu to set interfacial area models.This menu is available only for the Mixture and

Eulerian multiphase models.

interfacial-area

Specifies the interfacial area model for each pair of phases.

model-transition/

Enters the menu to set model transition mechanisms.

model-transition

Sets the VOF-to-DPM model transition mechanism.

numerics/

Enters the menu to set numerics models.This menu is available for multiphase models with

the sharp-dispersed and phase localized discretization interface modeling options (set in

define/models/multiphase/interface-modeling-options).

interphase-discretization/

Enters the menu to set interphase discretization models.

interphase-discr?

Enables/disables phase localized compressive scheme.

slope-limiter

Specifies the slope limiter to set a specific discretization scheme for each phase pair.

A value of  corresponds to first order upwind, a value of  corresponds to second order

upwind, a value of  applies the compressive scheme, and a value between  and

corresponds to a blended scheme.This option is available only when interphase-

discr? is enabled.

phase-domains/

Enters the menu to select a specific phase.

phasename/

Enters the menu for setting properties for the selected phase phasename, where phasename

is the name of the phase you selected using the phase-domains/ text command.

diameter

Sets the diameter of the particles of the selected phase phasename.This text command

is available for secondary phases only.

granular-properties/

Enters the menu for setting properties for the granular phase.This text command is available

only when the granular? text command is enabled.

bulk-viscosity

Sets the solids bulk viscosity (constant, lun-et-al, or user-defined).

elasticity-modulus

Specifies the elasticity modulus (derived or user-defined).

friction-angle

Sets the angle of internal friction (constant or user-defined).This text command is

available only when schaeffer is selected as the friction viscosity model.

friction-packing

Sets a threshold volume fraction at which the frictional regime becomes dominant

(constant or user-defined).The default value is ..This text command is available

only when schaeffer is selected as the friction viscosity model.

define/

friction-viscosity

Specifies a shear viscosity based on the viscous-plastic flow (none, constant, schaeffer,

or user-defined). By default, the frictional viscosity is neglected (none).

Note

When schaeffer is selected as the friction viscosity model, you

must specify friction-angle, friction-packing, friction-

al-modulus, and frictional-pressure.

frictional-modulus

Sets the frictional modulus (derived or user-defined).This text command is available

frictional-pressure

Sets the pressure gradient term in the granular-phase momentum equation (none,

johnson-et-al, syamlal-et-al, based-ktgf, or user-defined).This text command is available

granular-conductivity

Sets temperature for the solids phase (constant, syamlal-obrien, gidaspow, or user-

defined).This text command is available only if the pde-granular? text command

granular-temperature

Sets temperature for the solids phase (algebraic, constant, dpm-averaged, or user-

defined).The dpm-averaged option is available only when using the Dense Discrete

Phase Model (DDPM).This text command is available only if the pde-granular?

text command is disabled.

packed-bed?

Enables/disables the packed bed model.

packing

Sets the maximum volume fraction for the granular phase (constant or user-defined).

For monodispersed spheres the packing limit is about ..

pde-granular?

Enables/disables the partial differential equation (PDE) model for granular temperature.

When the PDE model is enabled, you must specify granular-conductivity.

Otherwise, you must specify granular-temperature.

radial-distribution

Sets a correction factor that modifies the probability of collisions between grains when

the solid granular phase becomes dense (lun-et-al, syamlal-obrien, ma-ahmadi,

arastoopour, or user-defined).

solids-pressure

Sets the pressure gradient term in the granular-phase momentum equation (lun-et-al,

syamlal-obrien, ma-ahmadi, user-defined, or none).

viscosity

Sets the kinetic part of the granular viscosity of the particles (constant, syamlal-obrien,

gidaspow, or user-defined).

granular?

Enables/disables the granular approach for the solid phase.This text command is available

only for secondary phases in a Eulerian multiphase case.This approach is not compatible

with the interfacial area concentration approach. For more details, see Defining a Granular

Secondary Phase in the Fluent User's Guide.

iac-properties/

Enters the menu for setting model properties for the interfacial area concentration.This

text command is available only when the iac? text command is enabled.

iac-breakage-kernel

Sets the breakage kernel (none, constant, hibiki-ishii, ishii-kim, yao-morel, or user-

defined).

iac-coalescence-kernel

Sets the coalescence kernel (none, constant, hibiki-ishii, ishii-kim, yao-morel, or user-

defined).

iac-critical-weber

Sets the critical Weber number.This value is required if you selected yao-morel as

the breakage kernel.

iac-dissipation-rate

Allows you to choose the dissipation function (constant, wu-ishii-kim, fluent-ke, or user-

defined).

iac-hydraulic-diam

Sets the hydraulic diameter.This value is required when you selected wu-ishii-kim

for the IAC dissipation rate function.

iac-max-diameter

Sets the maximum for the bubble diameters.

iac-min-diameter

Sets the minimum for the bubble diameters.

iac-nucleation-kernel

Sets the source term for the interfacial area concentration that models the rate of

formation of the dispersed phase (none, constant, yao-morel, or user-defined).

iac-surface-tension

Sets the attractive forces between the interfaces.

iac?

Enables/disables the interfacial area concentration (IAC) approach.This text command is

available for secondary phases only.The IAC approach is not compatible with the granular

approach. See Defining the Interfacial Area Concentration via the Transport Equation and

Defining the Interfacial Area Concentration in the Fluent User's Guide for details about using

the IAC approach for the Mixture and Eulerian multiphase flows.

define/

material

Sets a material for the selected phase.

profiles/

Enters the boundary profiles menu.

delete

Deletes a profile.

define/

material

profiles/

delete

Deletes all boundary-profiles.

interpolation-method

Chooses the method for interpolation of profiles.

link-profile-to-reference-frame

Attaches a profile to a reference frame so that the profile will rotate according to the reference frame.

list-profiles

Lists all profiles.

list-profile-fields

Lists the fields of a particular profile.

morphing?

Enables/disables profile morphing options in Orient Profile panel.

Sets interval between updates of dynamic profiles.

reference-frames/

Enters the reference frames menu.

add

Creates a new reference frame.

delete

Deletes the reference frame you specify.

display

Displays the reference frame you specify.

edit

Allows you to edit a reference frame.

hide

Removes the specified reference frame from the graphics window.

list

Lists all of the reference frames.

Lists the properties of the reference frame you specify.

set-unit-system

Applies a standard set of units to all quantities.The options include default, si, british, and cgs.

solution-strategy/

Enters the automatic initialization and case modification strategy menu.

automatic-case-modification/

Enters the automatic case modification menu.

before-init-modification

Specifies modification to be performed before initialization.

modifications

Specifies modifications to be performed during solution.

original-settings

Specifies modification to be performed after initialization to restore to original settings.

automatic-initialization

Defines how the case is to be automatically initialized.

continue-strategy-execution

Continues execution of the currently defined automatic initialization and case modification strategy.

enable-strategy?

Enables/disables automatic initialization and case modification.

execute-strategy

Executes the currently defined automatic initialization and case modification strategy.

turbo/

Enters the turbo menu.

define-topology

Defines a turbo topology.

mesh-method

Sets turbo structured mesh generation method.

search-method

Sets search method for a topology.

projection-method

Sets 2D projection method.

units

Sets unit conversion factors.

user-defined/

Enters the user-defined functions and scalars menu.

1D-coupling

Loads 1D library.

define/

compiled-functions

Opens user-defined function library.

execute-on-demand

Executes UDFs on demand.

fan-model

Configures user-defined fan model.

function-hooks

Hooks up user-defined functions.

interpreted-functions

Loads interpreted user-defined functions.

real-gas-models

Enters the real-gas menu to enable/configure real gas model.

nist-multispecies-real-gas-model

Loads the NIST real-gas library.

nist-real-gas-model

nist-settings

Specifies the name and the location for the REFPROP library and fluid files.

set-state

Selects the state for NIST real gas model.

user-defined-multispecies-real-gas-model

Loads a user-defined multispecies real-gas library.

user-defined-real-gas-model

Loads the user-defined real-gas library.

use-contributed-cpp?

Enables/disables use of the cpp utility included with the ANSYS Fluent installation.

user-defined-memory

Allocates user-defined memory.

user-defined-scalars

Defines user-defined scalars.

add-custom-vector

Adds new custom vector definition.

annotate

Adds annotation text to a graphics window. It will prompt you for a string to use as the annotation text,

mouse.

clear-annotations

Removes all annotations and attachment lines from the active graphics window.

close-window

Closes a graphics window.

contour

Prompts for a scalar field and minimum and maximum values, and then displays a contour plot.

display-custom-vector

Displays custom vector.

flamelet-data

Displays flamelet data.

carpet-plot

Enables/disables display of carpet plot of a property.

draw-number-box?

Enables/disables display of the numbers box.

plot-1d-slice?

Enables/disables plot of the 1D-slice.

write-to-file?

Enables/disables writing the 1D-slice to file instead of plot.

graphics-window-layout

Arranges the graphics window layout.

hsf-file

Loads an HSF file for viewing.

mesh

Displays the entire mesh. For 3D, you will be asked to confirm that you really want to draw the entire mesh

(not just the mesh-outline).

mesh-outline

Displays the mesh boundaries.

mesh-partition-boundary

Displays mesh partition boundaries.

multigrid-coarsening

Displays a coarse mesh level from the last multigrid coarsening.

objects

Enters the graphics objects menu.

Adds a contour, vector, pathline, particle track, scene, or mesh plot to the existing content in the

copy

objects

copy

Copies an existing contour, vector, pathline, particle track, scene, mesh, or XY plot definition.

create

Creates a contour, vector, pathline, particle track, scene, mesh, or XY plot definition.

delete

Deletes a contour, vector, pathline, particle track, scene, mesh, or XY plot definition.

display

Displays a contour, vector, pathline, particle track, scene, mesh, or XY plot in the graphic windows re-

placing the existing content.

edit

Edits a contour, vector, pathline, particle track, scene, or mesh plot definition.

open-window

Opens a graphics window.

particle-tracks/

Enters the particle tracks menu.

particle-tracks

Calculates and displays particle tracks from defined injections.

plot-write-xy-plot

Plots or writes an XY plot of particle tracks.

path-lines/

Enters the pathlines menu.

path-lines

Displays pathlines from a surface.

Plots or writes an XY plot of pathlines.

write-to-files

Writes pathlines to a file.

pdf-data/

Enters the PDF data menu.

display/

Enables/disables the display of a carpet plot of a property.

Enables/disables the display of the numbers box.

Enables/disables a plot of the 1D-slice.

reacting-channel-curves

Plots the reacting channel variables.

profile

Displays profiles of a flow variable.

re-render

Re-renders the last contour, profile, or vector plot with updated surfaces, meshed, lights, colormap, rendering

options, and so on, without recalculating the contour data.

re-scale

re-render

re-scale

Re-renders the last contour, profile, or vector plot with updated scale, surfaces, meshes, lights, colormap,

rendering options, and so on, but without recalculating the field data.

Generates a “hardcopy" of the active window.

set/

Enters the set menu to set display parameters.

color-map/

Enters the color map menu, which contains names of predefined and user-defined (in the Colormap

Editor panel) colormaps that can be selected. It prompts you for the name of the colormap to be used.

colors/

Enters the color options menu.

Sets the color of axisymmetric faces.

Sets the background (window) color.

Determines whether to color meshes by type or by ID.

Sets the color of far field faces.

Sets the color of free-surface faces.

Sets the color theme for the graphics window.The color options are for the background display,

but changing the theme also changes the default colors for items that display in the graphics

windows, like faces and edges.

Sets the foreground (text, ruler, and window frame) color.

Sets highlight color.

Sets the color of inlet faces.

Sets the color of mesh interfaces.

Sets the color of interior faces.

Sets the color of internal interface faces.

Sets the color of outlet faces.

Sets the color of periodic faces.

Sets the color of RANS/LES interface faces.

Sets the color of symmetric faces.

Sets the color of traction faces.

Sets the color of wall faces.

list

Lists available colors.

Resets individual mesh surface colors to the defaults.

Sets the number of labels to be skipped in the colormap scale.

surface

Sets the color of surfaces.

contours/

Enters the contour options menu.

display/

auto-range?

Enables/disables auto-computation of the contour range.

clip-to-range?

Turns the clip to range option for filled contours on/off.

coloring

Specifies whether contours are displayed in bands or with smooth transitions. Note that you can

only display smooth contours if node-values are enabled.

contour-lines?

With the filled-contours? and node-values? options enabled, this sets the use of lines

to delineate the bands of color to coincide with the colormap.

filled-contours?

Turns the filled contours option on/off (deselects line-contours? ).

global-range?

Turns the global range for contours on/off.

line-contours?

Turns the line contours option on/off (deselects filled-contours? ).

log-scale?

Specifies a decimal or logarithmic color scale for contours.

n-contour

Sets the number of contour levels.

node-values?

Sets the option to use scalar field at nodes when computing the contours.

render-mesh?

Determines whether or not to render the mesh on top of contours, vectors, and so on.

surfaces

Sets the surfaces on which contours are drawn.You can include a wildcard (*) within the surface

names.

element-shrink

surfaces

names.

Sets shrinkage of both faces and cells. A value of zero indicates no shrinkage, while a value of one will

shrink each face or cell to a point.

filled-mesh?

Determines whether the meshes are drawn as wireframe or solid.

mesh-level

Sets coarse mesh level to be drawn.

mesh-partitions?

Enables/disables option to draw mesh partition boundaries.

mesh-surfaces

Sets surface IDs to be drawn as meshes.You can include a wildcard (*) within the surface names.

mesh-zones

Sets zone IDs to be drawn as meshes.

picture/

Enters the save-picture options menu.

Enters the hardcopy/save-picture color mode menu.

color

Plots hardcopies in color.

Converts color to grayscale for hardcopy.

list

Displays the current hardcopy color mode.

Converts color to monochrome (black and white) for hardcopy.

Sets the width of raster-formatted images in pixels ( implies current window size).

Sets the height of raster-formatted images in pixels ( implies current window size).

dpi

Sets the resolution for EPS and Postscript files; specifies the resolution in dots per inch (DPI) instead

of setting the width and height.

driver/

Enters the set hardcopy driver menu.

Sets the command used to dump the graphics window to a file.

eps

Produces encapsulated PostScript (EPS) output for hardcopies.

hsf

Produces HOOPS Visualize Stream Format (HSF) output for hardcopies.

jpeg

Produces JPEG output for hardcopies. (This is the default file type.)

list

Lists the current hardcopy driver.

options

jpeg

list

options

Sets the hardcopy options. Available options are:“no gamma correction", disables gamma correction

of colors;“pen speed = f", where f is a real number in [,];“physical size = (width, height)", where

width and height are the actual measurements of the printable area of the page in centimeters;

“subscreen = (left, right, bottom, top)", where left, right, bottom, and top are numbers in [-,]

display/

describing a subwindow on the page in which to place the hardcopy.The options may be combined

by separating them with commas.The pen speed option is only meaningful to the HPGL driver.

png

Uses PNG output for hardcopies.

Enters the PostScript driver format menu.

Enables a raster file that may be larger than the standard raster file, but will print much more

quickly.

raster

Enables the standard raster file.

Enables a run-length encoded raster file that will be about the same size as the standard raster

file, but will print slightly more quickly.

vector

Enables the standard vector file.

Produces PostScript output for hardcopies.

ppm

Produces PPM output for hardcopies.

tiff

Produces TIFF output for hardcopies.

vrml

Uses VRML output for hardcopies.

Exchanges foreground/background colors for hardcopy.

Plots hardcopies in landscape or portrait orientation.

Controls the size and quality of how JPEG files are saved based on a scale of -, with zero being

preview

preview

Applies the settings of the color-mode, invert-background, and landscape options to the currently

Disables/enables the use of the current graphics window resolution when saving an image of the

graphics window. If disabled, the resolution will be as specified for x-resolution and y-resolu-

tion.

lights/

Enters the lights menu.

Turns the light that moves with the camera on or off.

Sets lighting interpolation method.

flat

Uses flat shading for meshes and polygons.

gouraud

Uses Gouraud shading to calculate the color at each vertex of a polygon and interpolates it in

the interior.

phong

Uses Phong shading to interpolate the normals for each pixel of a polygon and computes a

color at every pixel.

Turns all active lighting on/off. This command is only available when the headlight-on? option

is turned off (lights-on? is enabled when the headlight is on).

Sets the ambient color for the scene.The ambient color is the background light color in a scene.

set-light

Adds or modifies a directional, colored light.

Sets the line-weight factor for the window.

marker-size

Sets the size of markers used to represent points.

marker-symbol

Sets the type of markers used to represent points.

mesh-display-configuration

Changes the default mesh display. If set to meshing, it draws the mesh on edges and faces of the

outline surfaces, colored by their zone ID with lighting enabled. If set to solution, it draws the mesh

on edges and faces of the outline surfaces, colored by their zone type with lighting enabled. If set to

post-processing, it draws the object outline with lighting disabled. If set to classic, it draws the mesh

on all edges of the outline surfaces.

Note

This only applies for 3D cases.

mirror-zones

Sets the zones about which the domain is mirrored (symmetry planes).

display/

Prompts you to select a function for each of the mouse buttons.

mouse-probes?

Enables/disables mouse probe capability.

n-stream-func

Sets number of iterations used in computing stream function.

nodewt-based-interp?

Disables/enables the use of node weights for node-based gradients in postprocessing.

overlays?

Enables/disables overlays.

Enters the particle-tracks menu to set parameters for display of particle tracks.

arrow-scale

Sets the scale factor for arrows drawn on particle tracks.

arrow-space

Sets the spacing factor for arrows drawn on particle tracks.

coarsen-factor

Sets the coarsening factor for particle tracks.

display?

Determines whether particle tracks shall be displayed or only tracked.

filter-settings/

Sets filter for particle display.

enable-filtering?

Specifies whether particle display is filtered.

filter-variable

Selects a variable used for filtering of particles.

inside?

Specifies whether filter variable must be inside min/max to be displayed (else outside min/max).

maximum

Specifies the upper bound for the filter variable.

inside?

maximum

minimum

Specifies the lower bound for the filter variable.

history-filename

Specifies the name of the particle history file.

line-width

Sets the width for particle track.

Sets the size of markers used to represent particle tracks.

particle-skip

Specifies how many particle tracks should be displayed.

radius

Sets the radius for particle track (ribbon/cylinder only) cross-section.

report-to

Specifies the destination for the report (console, file, none).

report-type

Sets the report type for particle tracks.

report-variables

Sets the report variables.

report-default-variables

Sets the report variables to default.

sphere-attrib

Specifies the size and number of slices to be used in drawing spheres.

sphere-settings/

Specifies whether displayed spheres should include auto range of variable to size spheres.

diameter

Diameter of the spheres when vary-diameter is disabled.

maximum

Sets the maximum value of the sphere to be displayed.

minimum

Sets the minimum value of the sphere to be displayed.

scale-factor

Specifies a scale factor to enlarge/reduce the size of spheres.

size-variable

Selects a particle variable to size the spheres.

smooth-parameter

Specifies number of slices to be used in drawing spheres.

vary-diameter?

Specifies whether the spheres can vary with another variable.

style

Sets the display style for particle track (line/ribbon/cylinder/sphere).

display/

track-single-particle-stream?

Specifies the stream ID to be tracked.

twist-factor

Sets the scale factor for twisting (ribbons only).

display/

vector-settings/

Sets vector specific input.

color-variable?

Specifies whether the vectors should be colored by variable specified in /display/particle-

track/particle-track (if false use a constant color).

constant-color

Specifies a constant color for the vectors.

length-to-head-ratio

Specifies ratio of length to head for vectors and length to diameter for cylinders.

length-variable?

Specifies whether the displayed vectors have length varying with another variable.

Specifies a scale factor to enlarge/reduce the length of vectors.

style

Enables and sets the display style for particle vectors (none/vector/centered-vector/centered-

cylinder).

vector-length

Specifies the length of constant vectors.

vector-length-variable

Selects a particle variable to specify the length of vectors.

vector-variable

Selects a particle vector function to specify vector direction.

Sets parameters for display of pathlines.

Sets the scale factor for arrows drawn on pathlines.

Sets the spacing factor for arrows drawn on pathlines.

display-steps

Sets the display stepping for pathlines.

Sets error control during pathline computation.

Sets the width for pathlines.

Sets the marker size for particle drawing.

maximum-error

Sets the maximum error allowed while computing the pathlines.

maximum-steps

Sets the maximum number of steps to take for pathlines.

radius

Sets the radius for pathline (ribbons/cylinder only) cross-section.

relative-pathlines?

Enables/disables the tracking of pathlines in a relative coordinate system.

radius

reverse?

Sets direction of path tracking.

step-size

Sets the step length between particle positions for pathlines.

style

Selects the pathline style (line, point, ribbon, triangle, cylinder).

time-step

Sets the time step between particle positions for pathlines.

track-in-phase

Selects the phase in which particle pathlines will be computed (Multiphase Eulerian Model only).

periodic-repeats

Sets number of periodic repetitions.

proximity-zones

Sets zones to be used for boundary cell distance and boundary proximity.

Enables/disables rendering the mesh on top of contours, vectors, and so on.

rendering-options

Enters the rendering options menu, which contains the commands that allow you to set options that

determine how the scene is rendered.

Uses of wireframe or all during animation.

Enables/disables mouse view rotations to continue to spin the display after the button is released.

display/

Sets the color bar alignment.

Prints out information about your graphics driver.

Enables/disables double buffering. Double buffering dramatically reduces screen flicker during

driver

driver

Note

Sets face displacement value in Z-buffer units along the Camera Z-axis.

hidden-line-method

Specifies the method to perform hidden line rendering.This command will appear only when

hidden-lines? is true.

Normal hidden lines algorithm.This is the default.

For removing hidden lines for surfaces that are very close together. Use this if normal-hlr-

algorithm is not working.This will only work for meshes.

Note

Turns hidden line removal on/off.

Note

Turns hidden surface removal on/off.

Allows you to choose from among the hidden surface removal methods that ANSYS Fluent supports.

These options (listed below) are display hardware dependent.

Is the fastest method if your hardware supports it.The accuracy and speed of this method is

painters

Will show less edge-aliasing effects than hardware-z- buffer.This method is often used instead

Is the fastest of the accurate software methods available (especially for complex scenes), but

Is a fast software method, but it is not as accurate as software-z-buffer.

Enables/disables discarding outer faces during display.

Sets the rendering options.

Sets edge visibility flags for surfaces.

Resets the graphics system.

title

Sets problem title.This text only appears if the display/set/windows/text/company? text

command is set to yes and if Titles is enabled in the Display Options dialog box.

left-top

Sets the title text for left top in title segment.

left-bottom

Sets the title text for left bottom in title segment.

right-top

Sets the title text for right top in title segment.

right-middle

Sets the title text for right middle in title segment.

right-bottom

Sets the title text for right bottom in title segment.

velocity-vectors/

Enters the menu to set parameters for display of velocity vectors.

display/

Auto-scales all vectors so that vector overlap is minimal.

color

Sets the color of all velocity vectors to the color specified.The color scale is ignored.This is useful

when overlaying a vector plot over a contour plot.

color-levels

color

Sets the number of colors used from the colormap.

component-x?

Sets the option to use only the  component of the velocity vectors during display.

component-y?

component-z?

constant-length?

Sets the option to draw velocity vectors of constant length.This shows only the direction of the

velocity vectors.

Turns global range for vectors on/off.

in-plane?

Toggles the display of velocity vector components in the plane of the surface selected for display.

Toggles whether color scale is logarithmic or linear.

Enables/disables the plotting of node values. Cell values will be plotted if "no".

relative?

Toggles the display of relative velocity vectors.

scale

Sets the value by which the vector length will be scaled.

scale-head

Sets the value by which the vector head will be scaled.

style

Specifies the vector style that will be used when the vectors are displayed.You can choose from:

3d arrow, 3d arrowhead, cone, filled-arrow, arrow, harpoon, or headless.

surfaces

Sets surfaces on which vectors are drawn.You can include a wildcard (*) within the surface names.

windows/

Enters the windows option menu, which contains commands that allow you to customize the relative

positions of subwindows inside the active graphics window.

Sets the aspect ratio of the active window.

axes/

axes/

Enters the axes window options menu (3D only).

border?

Sets whether to draw a border around the axes window.

bottom

Sets the bottom boundary of the axes window.

clear?

Sets the transparency of the axes window.

logo?

Enables/disables visibility of the logo in graphics window.

logo-color

Sets logo color to white/black in graphics window.

right

Sets the right boundary of the axes window.

visible?

Turns axes visibility on/off.

main/

Enters the main view window options menu.

border?

Sets whether or not to draw a border around the main viewing window.

bottom

Sets the bottom boundary of the main viewing window.

left

Sets the left boundary of the main viewing window.

right

Sets the right boundary of the main viewing window.

top

Sets the top boundary of the main viewing window.

visible?

Turns visibility of the main viewing window on/off.

ruler?

Turns the ruler on/off. Note that if you are running Fluent in 3D, then the view must be set to or-

thographic.

display/

scale/

Enters the color scale window options menu.

alignment

Sets the colormap position to the bottom, left, top, or right.

border?

Sets whether or not to draw a border around the color scale window.

bottom

Sets the bottom boundary of the color scale window.

clear?

Sets the transparency of the scale window.

format

Sets the number format of the color scale window. (for example, %.2e)

font-size

Sets the font size of the color scale window.

left

Sets the left boundary of the color scale window.

margin

Sets the margin of the color scale window.

right

Sets the right boundary of the color scale window.

top

left

margin

right

top

Sets the top boundary of the color scale window.

visible?

Turns visibility of the color scale window on/off.

text/

Enters the text window options menu.

Shows/hides the application name in the picture.

border?

Sets whether or not to draw a border around the text window.

bottom

Sets the bottom boundary of the text window.

clear?

Enables/disables text window transparency.

company?

Enables/disables the display of your company name or other text defined using the dis-

play/set/titles/ text command.The text appears in the title box. See Controlling the

Titles, Axes, Ruler, Logo, and Colormap in the Fluent User's Guide for additional information.

date?

Shows/hides the date in the picture.

left

Sets the left boundary of the text window.

right

Sets the right boundary of the text window.

top

Sets the top boundary of the text window.

visible?

Turns visibility of the text window on/off.

video/

Enters the video window options menu.

Sets the background color of the graphics window.The color is specified as a string of three

to change the background from black (default) to gray, you would enter ".,.,." after

selecting the background command.

Sets the video color filter. For example, to change the color filter from its default setting to PAL

Sets the foreground (text) color of the graphics window.The color is specified as a string of

ample, to change the foreground from white (default) to gray, you would enter ".,.,."

after selecting the foreground command.

on?

Enables/disables video picture settings.

Sets the window size in pixels.

xy/

Enters the XY plot window options menu.

border?

Sets whether or not to draw a border around the XY plot window.

bottom

Sets the bottom boundary of the XY plot window.

left

Sets the left boundary of the XY plot window.

right

Sets the right boundary of the XY plot window.

display/

top

Sets the top boundary of the XY plot window.

visible?

Turns visibility of the XY plot window on/off.

zero-angle-dir

Sets the vector having zero angular coordinates.

Sets the separator character for list tree.

set-window

Sets a graphics window to be the active window.

surface/

Enters the data surface-manipulation menu. For a description of the items in this menu, see sur-

face/ (p. ).

surface-cells

Draws the cells on the specified surfaces.You can include a wildcard (*) within the surface names.

surface-mesh

Draws the mesh defined by the specified surfaces.You can include a wildcard (*) within the surface names.

Enters the scene options menu.

delete

Deletes selected geometries.

display

Displays selected geometries.

Enables/disables drawing the bounding frame.

iso-sweep

Changes iso-sweep values.

overlays?

Enables/disables the overlays option.

pathline

display

iso-sweep

overlays?

pathline

Changes pathline attributes.

Selects geometry to be updated.

set-frame

Changes frame options.

time

Changes time-step value.

transform

Applies transformation matrix on selected geometries.

vector

Displays vectors of a space vector variable.

velocity-vector

Prompts for a scalar field by which to color the vectors, the minimum and maximum values, and the scale

factor, and then draws the velocity vectors.

view/

Enters the view manipulation menu. For a description of the items in this menu, see views/ (p. ).

zone-mesh

Draws the mesh defined by specified face zones. Zone names can be indicated using wildcards (*).

display/

Chapter : exit / close-fluent

exit

Exits program.

close-fluent

(ANSYS Fluent in Workbench only) Exits program.

async-optimize?

Chooses whether to optimize file I/O using scratch disks and asynchronous operations.

auto-save/

Enters the auto save menu.

append-file-name-with

Sets the suffix for auto-saved files.The file name can be appended by flow-time, time-step value, or

by user-specified flags in file name.

case-frequency

Specifies the frequency (in iterations, time steps, or flow time) with which case files are saved.

data-frequency

Specifies the frequency (in iterations, time steps, or flow time) with which data files are saved.

max-files

Sets the maximum number of files. Once the maximum is reached, files will be erased as new files are

written.

overwrite-existing-files

Overwrites existing files when files are automatically saved.

retain-most-recent-files

written.

Sets autosave to retain the  most recent files.

root-name

Specifies the root name for the files that are saved.

save-data-file-every

Specifies the type and frequency of the data file to be saved.

binary-files?

Indicates whether to write binary or text format case and data files.

close-without-save?

Exits ANSYS Fluent without saving data in Workbench.This command is only available when running ANSYS

Fluent in Workbench.

Confirms attempts to overwrite existing files.

data-file-options

Sets derived quantities to be written in data file.

define-macro

Saves input to a named macro.

em-mapping

Enters the electromagnetic loss mapping menu.

Important

When ANSYS Fluent is run under Workbench and a connection is detected between the

ANSYS Fluent and ANSYS Maxwell applications, the em-mapping text command menu

includes only the volumetric-energy-loss and surface-energy-loss com-

mands. The maintain-loss-on-initialization and remove-loss-only

commands are available when there is no connection between ANSYS Fluent and ANSYS

Maxwell and Fluent has electromagnetic loss data; Fluent can receive this loss data

through a connection or from a previously solved data file.

maintain-loss-on-initialization

Maintains the loss data provided by Maxwell even if solution is initialized.

remove-loss-only

Removes the loss data provided by Maxwell and keeps all other solution data.

surface-energy-loss

Maps the total surface loss (that is, heat source) from Maxwell to ANSYS Fluent so that you can perform

a thermal analysis.This option is only available when there is a connection detected between the

ANSYS Fluent and Maxwell applications.

volumetric-energy-loss

Maps the total volumetric loss (that is, heat source) from Maxwell to ANSYS Fluent so that you can

perform a thermal analysis.This option is only available when there is a connection detected between

the ANSYS Fluent and Maxwell applications.

execute-macro

Runs a previously defined macro.

export-to-cfd-post

Exports data files that are compatible with CFD-Post and EnSight (that is, .cdat and .cst files) and opens

CFD-Post, if desired.

export/

Exports case and data information.

abaqus

Writes an ABAQUS file.

ascii

Writes an ASCII file.

avs

Writes an AVS UCD file.

cdat-for-cfd-post-&-ensight

Writes data files that are compatible with CFD-Post and EnSight (that is, .cdat and .cst files).

cgns

Writes a CGNS file.

file/

custom-heat-flux

Writes a generic file for heat transfer.

dx

Writes an IBM Data Explorer format file.

ensight

Writes EnSight geometry, velocity, and scalar files.

ensight-gold

Writes EnSight Gold geometry, velocity, and scalar files.

ensight-gold-parallel-surfaces

Writes EnSight Gold geometry, velocity, and scalar files for surfaces in a parallel format suitable for

EnSight Enterprise.

ensight-gold-parallel-volume

Writes EnSight Gold geometry, velocity, and scalar files for cell zones in a parallel format suitable for

ensight-gold-transient

Writes EnSight Gold Transient geometry, velocity, and scalar files.

fast-mesh

Writes FAST/Plot3D unstructured mesh file.

fast-scalar

Writes FAST/Plot3D unstructured scalar function file.

fast-solution

Writes FAST/Plot3D unstructured solution file.

fast-velocity

Writes FAST/Plot3D unstructured vector function file.

fieldview

Writes FIELDVIEW case and data files.

fieldview-data

fieldview-unstruct

Writes FIELDVIEW unstructured combined file.

fieldview-unstruct-mesh

Writes FIELDVIEW unstructured mesh-only file.

fieldview-unstruct-data

Writes FIELDVIEW unstructured results-only file.

fieldview-unstruct-surfaces

Writes FIELDVIEW unstructured file for surfaces.You are prompted to select either [], [] or [] to

write either mesh-only, results-only, or combined for surfaces (respectively).

gambit

Writes GAMBIT neutral file.

icemcfd-for-icepak

Writes a binary ICEM CFD domain file.

ideas

Writes an I-deas universal file.

mechanical-apdl-input

Writes a Mechanical APDL Input file.

nastran

Writes a NASTRAN file.

particle-history-data

Exports particle-history data.

patran-neutral

Writes a PATRAN neutral file.

patran-nodal

Writes a PATRAN nodal results file.

system-coupling-definition-file-settings/

Enters the system coupling file (.scp) menu.

enable-automatic-creation-of-scp-file

enables/disables automatically writing a .scp every time a case file is written.

write-system-coupling-file

Writes a system coupling (.scp) file.

taitherm

Exports TAITherm file.

tecplot

Writes a Tecplot+3DV format file.

fsi/

Enters the fluid-structure interaction menu.

display-fsi-mesh

Displays the mesh for a fluid-structure interaction.

read-fsi-mesh

Reads an FEM mesh for one-way data mapping from ANSYS Fluent.

write-fsi-mesh

Writes a fluid-structure interaction mesh file.

hdf-files?

Answering yes will set HDF5 as the default file format for reading and writing case/data files.

file/

hdfio-options/

Enters the HDF options menu

compression-level

Sets the compression level for HDF-formatted files.The compression level can be set between  and

with  being no compression (fastest) and  being highest compression (slowest).

io-mode

Sets the I/O mode for writing HDF files.

HOST: I/O is done serially by the host process.

NODE0: I/O is done serially by the node  process.

PARALLEL INDEPENDENT: I/O is done in parallel using the independent mode of MPI I/O.

PARALLEL COLLECTIVE: I/O is done in parallel using the collective mode of MPI I/O.

single-precision-data?

Specifies whether the double-precision solver saves single-precision data when writing HDF data files,

in order to reduce the size of the files.

import/

Imports case and data information.

abaqus/

Imports an ABAQUS file.

fil

Reads an ABAQUS .fil result file as a case file.

input

Reads an ABAQUS input file as a case file.

odb

Reads an ABAQUS odb file as a case file.

cfx/

Imports a CFX file.

definition

Reads a CFX definition file as a case file.

result

cgns/

Imports a CGNS file.

data

Reads data from CGNS file.

mesh

Imports a CGNS mesh file.

mesh-data

Imports a CGNS mesh file and data file.

chemkin-mechanism

Reads a CHEMKIN mechanism file.

chemkin-report-each-line?

Enables/disables reporting after reading each line.

ensight

Reads an EnSight file as a case file.

fidap

Imports a FIDAP neutral file.

flamelet/

Imports a flamelet file.

standard

ensight

fidap

flamelet/

standard

Reads a standard format flamelet file.

cfx-rif

Reads a CFX-RIF format flamelet file.

fluent4-case

Imports a formatted ANSYS Fluent  case file.

gambit

Imports a GAMBIT neutral file.

hypermesh

Reads a HYPERMESH file as a case file.

ideas-universal

Imports an I-deas Universal file.

lstc/

Imports an LSTC file.

input

Reads an LSTC input file as a case file.

state

Reads an LSTC result file as a case file.

marc-post

Reads a MARC POST file as a case file.

mechanical-apdl/

Imports a Mechanical APDL file.

input

Reads a Mechanical APDL file as a case file.

result

Reads a Mechanical APDL result file as a case file.

file/

nastran/

Imports a NASTRAN file.

bulkdata

Reads a NASTRAN file as a case file.

output2

Reads a NASTRAN op2 file as a case file.

partition/

Enters the partition menu to set conditions for partitioning an ANSYS Fluent case file during read.

metis

Reads and partitions an ANSYS Fluent case file.

metis-zone

patran/

Imports a PATRAN neutral file (zones defined by named components).

neutral

Reads a PATRAN Neutral file (zones defined by named components) as a case file.

plot3d/

Imports a PLOT3D file.

mesh

Reads a PLOT3D file as a case file.

tecplot

Enters the Tecplot menu.

mesh

Reads a Tecplot binary file as a case file.

prebfc-structured

Imports a formatted PreBFC structured mesh file.

ptc-mechanica

Reads a PTC Mechanica Design file as a case file.

Loads the ANSYS ACT simulation customization tool.

interpolate/

Interpolates data to/from another grid.

read-data

read-data

Reads and interpolates data.

write-data

Writes data for interpolation.

zone-selection

Defines a list of cell zone IDs. If specified, interpolation data will be read/written for these cell zones

only.

read-case

Reads a case file.

read-case-data

Reads a case and a data file.

read-data

Reads a data file.

read-field-functions

Reads custom field function definitions from a file.

read-injections

Reads all DPM injections from a file.

read-isat-table

Reads ISAT Table.

Reads command input from one or more files.

read-macros

Reads macro definitions from a file.

read-pdf

Reads a PDF file.

read-profile

Reads boundary profile data.

read-rays

Reads a ray file.

read-settings

Reads and sets boundary conditions from a specified file.

read-surface-clusters

Reads surface clusters from a file.

read-transient-table

Reads table of transient boundary profile data.

read-viewfactors

Reads view factors from a file.

reload-setup

Discards any changes in the current ANSYS Fluent in Workbench session and removes any corresponding

data from the Solution cell.This command is only available when running ANSYS Fluent in Workbench.

replace-mesh

Replaces the mesh with a new one while preserving settings.

file/

set-batch-options

Sets the batch options.

added to a journal file as soon as you start the recording.

Displays current release and version information.

single-precision-coordinates?

Specifies whether the nodal coordinates should be written in single precision (rather than the default

double precision).This text command is only available in the single-precision version of ANSYS Fluent.

solution-files/

Enters the solution files menu.

delete-solution

Deletes solution files.

load-solution

Loads a solution file.

print-solution-files

Prints a list of available solution files.

Starts recording all input in a file. Note that commands entered using paths from older versions of Fluent

will be upgraded to their current path in the journal file.

Starts recording input and output in a file.

Stops recording input and closes journal file.

stop-macro

Stops recording input to a macro.

Stops recording input and output and closes transcript file.

sync-workbench

Directly updates Workbench with the most recent Fluent changes.This command is only available when

running ANSYS Fluent in Workbench.

transient-export/

abaqus

ascii

avs

cgns

dx

ensight-gold-from-existing-files

cgns

dx

Writes EnSight Gold files using ANSYS Fluent case files.

fast

Writes a FAST/Plot3D unstructured mesh velocity scalar file.

Writes a FAST/Plot3D unstructured solution file.

Writes a FIELDVIEW unstructured combined file.

Writes a FIELDVIEW unstructured mesh only file.

Writes a FIELDVIEW unstructured results only file.

Writes FIELDVIEW unstructured combined file for surfaces.

ideas

Writes a Mechanical APDL input file.

nastran

file/

taitherm

Writes a TAITherm file.

Sets up an automatic particle-history data export.

edit

Edits transient exports.

delete

Deletes transient exports.

settings/

Enters the automatic export settings menu.

cfd-post-compatible

Specifies when case files are written with the .cdat and .cst files exported for ANSYS CFD-Post.

Note that this setting is ignored if the Write Case File Every Time option is enabled in the Auto-

matic Export dialog box.

write-boundary-mesh

Writes the boundary mesh to a file.

Writes a case file.

write-case-data

Writes a case and a data file.

write-cleanup-script

Writes the cleanup-script-file for ANSYS Fluent.

Writes a data file.

write-fan-profile

Computes radial profiles for a fan zone and writes them to a profile file.

write-field-functions

Writes the currently defined custom field functions to a file.

write-flamelet

Writes a flamelet file.

write-injections

Writes out selected DPM injections to a file.

write-isat-table

Writes ISAT Table.

write-macros

Writes the currently defined macros to a file.

write-merge-profiles

Writes a .csv file with the selected surfaces consolidated into one set of data points.

write-pdat?

Enables / disables the attempt to save .pdat files. Note that this text command is no longer supported.

write-pdf

Writes a pdf file.

write-profile

Writes surface data as a boundary profile file.

write-settings

Writes out current boundary conditions in use.

write-surface-clusters/

Writes the surface clusters to a file.

Sets the parameters needed for the view factor calculations.

Sets the split angle for the clustering algorithm.

write-surface-clusters

Computes and writes surface clusters for S2S radiation model.

file/

adapt/

Enters the mesh adaption menu.

adapt-mesh

Adapts the mesh according to the methods and settings that you specified.

cell-registers/

Enters the cell registers menu.

add

Creates a new cell register.

apply-poor-mesh-numerics

Applies poor mesh numerics to the mesh of a cell register.

add

coarsen

Coarsen the mesh based on a cell register.

delete

Deletes a cell register.

display

Displays a cell register.

edit

Edits an existing cell register.

list

Lists all of the currently defined cell registers.

Lists the properties of a cell register.

refine

Refine the mesh based on a cell register.

coarsening-criteria

Allows you to provide an expression for the coarsening criterion.

display-adaption-cells

Displays the cells that are marked for adaption in the graphics window.

free-hierarchy

Deletes the defined adaption hierarchy.

geometry

Enters the geometry menu.

list-adaption-cells

Prints the number of cells marked for refinement, coarsening, and both to the console.

refinement-criteria

Allows you to provide an expression for the refinement criterion.

revert-to-R19.-user-interface

Reverts the user interface, specifically the Adapt group box of the Domain ribbon tab to contain the

same adaption register options as were available with ANSYS Fluent release .. Note that you cannot

"undo" this command once you enter it.

set/

Enters the set menu.

additional-refinement-layers

Allows you to specify additional refinement layers (this is an advanced control).

display-settings

Sets the graphics display options for the refinement, coarsening, and common cells.

dynamic-adaption?

Enables automatic mesh adaption during the calculation, based on your specified refinement and

coarsening settings.

dynamic-adaption-frequency

Specifies the interval for how many iterations or time steps must pass between two consecutive

automatic mesh adaptions.

maximum-refinement-level

Controls the number of levels of refinement used to split cells during the adaption.

method

minimum-cell-quality

diverges, you may find that using a higher minimum quality value resolves the issue.This text

command is only available for PUMA 3D adaption (that is, when you have entered ad-

apt/set/method ).

minimum-cell-volume

Restricts the size of cell that Fluent considers for refinement. Even if the cell is marked for refinement,

it will not be refined if its cell volume is less than this threshold value.

verbosity

Allows you set how much information about the adaption is printed to the console.

mesh/

adjacency

Views and renames face zones adjacent to selected cell zones.

check

Performs various mesh consistency checks and displays a report in the console that lists the domain extents,

the volume statistics, the face area statistics, and any warnings, as well as details about the various checks

and mesh failures (depending on the setting specified for mesh/check-verbosity).

check-verbosity

Sets the level of details that will be added to the mesh check report generated by mesh/check. A value

of  (the default) notes when checks are being performed, but does not list them individually. A value of

lists the individual checks as they are performed. A value of  lists the individual checks as they are per-

formed, and provides additional details (for example, the location of the problem, the affected cells).

The check-verbosity text command can also be used to set the level of detail displayed in the

mesh quality report generated by mesh/quality. A value of  (the default) or  lists the minimum

orthogonal quality and the maximum aspect ratio. A value of  adds information about the zones

that contain the cells with the lowest quality, and additional metrics such as the maximum cell

squish index and the minimum expansion ratio.

Reports solver memory use.

mesh-info

Prints zone information size.

Enters the zone modification menu. For a description of the items in this menu, see define/boundary-

conditions/modify-zones.

polyhedra/

Enters the polyhedra menu.

convert-domain

Converts the entire domain to polyhedra cells.

convert-hanging-nodes

Converts cells with hanging nodes/edges to polyhedra.

convert-skewed-cells

Converts skewed cells to polyhedra.

options/

Enters the polyhedra options menu.

migrate-and-reorder?

Enables / disables the migration of newly created partitions to the compute-nodes and the reorder-

ing of the domain as part of polyhedra conversion.This is disabled by default, because it requires

significant additional memory; when disabled, it is recommended that you save the case file after

conversion, read it in a new Fluent session (so that the new / stored partitions become active), and

then manually reorder using the mesh/reorder/reorder-domain text command. If you want

to run the calculation in the current Fluent session you can enable the migrate-and-reorder?

text command prior to conversion, but you must ensure that no more than half of the available

memory of your system is currently used.

preserve-boundary-layer?

Specifies whether boundary layer cells will be preserved when the domain is converted to polyhedra.

When the value is set to  (default) ANSYS Fluent checks for high aspect ratio cells at the boundary

layer and if any are found, Fluent asks if you want to preserve the boundary layer.When the value

is set to , the boundary layer cells are never preserved; when it is set to , the boundary layer cells

are always preserved (regardless of the aspect ratio of the boundary layer cells).

preserve-interior-zones

Enables the preservation of surfaces (that is, manifold zones of type interior) during the conversion

of the domain to polyhedra. Note that only those zones with a name that includes the string you

specify will be preserved.

quality

Displays information about the quality of the mesh in the console, including the minimum orthogonal

quality and the maximum aspect ratio.The level of detail displayed depends on the setting specified for

mesh/check-verbosity.

redistribute-boundary-layer

Redistributes the nodes in a boundary layer zone to achieve a desired growth rate after anisotropic adaption.

reorder/

Reorders domain menu.

band-width

Prints cell bandwidth.

reorder-domain

Reorders cells and faces using the reverse Cuthill-McKee algorithm. Note that you must save a new

case file (and a data file, if data exists) after reordering with this text command, as well as recreate any

ray files and/or surface cluster information.

reorder-zones

Reorders zones by partition, type, and ID.

repair-improve

allow-repair-at-boundaries

Allows the adjustment of the positions of nodes on boundaries as part of the mesh repairs performed

by the mesh/repair-improve/repair text command.

Improves poor quality cells in the mesh, if possible.

include-local-polyhedra-conversion-in-repair

Enables/disables the local conversion of degenerate cells into polyhedra based on skewness criteria

as part of the mesh repairs performed by the mesh/repair-improve/repair text command.

repair

Repairs mesh problems identified by the mesh check, if possible.The repairs include fixing cells that

have the wrong node order, the wrong face handedness, faces that are small or nonexistent, or very

poor quality. Only interior nodes are repositioned by default; boundary nodes may be repositioned if

the mesh/repair-improve/allow-repair-at-boundaries text command is enabled. Note

that highly skewed cells may be converted into polyhedra, depending on whether the mesh/repair-

improve/include-local-polyhedra-conversion-in-repair text command is enabled.

mesh/

Modifies cell centroids to repair meshes that contain left-handed faces without face node order prob-

lems.

repair-face-node-order

Modifies face nodes to repair faces with improper face node order and, therefore, eliminates any res-

ulting left-handed faces.

repair-periodic

Modifies the mesh to enforce a rotational angle or translational distance for periodic boundaries. For

translationally periodic boundaries, the command computes an average translation distance and adjusts

the node coordinates on the shadow face zone to match this distance. For rotationally periodic

boundaries, the command prompts for an angle and adjusts the node coordinates on the shadow face

zone using this angle and the defined rotational axis for the cell zone.

repair-wall-distance

Corrects wall distance at very high aspect ratio hexahedral/polyhedral cells.

report-poor-elements

Reports invalid and poor quality elements.

rotate

Rotates the mesh.

scale

Prompts for the scaling factors in each of the active Cartesian coordinate directions.

size-info

Prints mesh size.

Smooths the mesh using quality-based, Laplacian, or skewness methods.

surface-mesh/

Enters the Surface Mesh menu.

delete

Deletes surface mesh.

display

Displays surface meshes.

read

Reads surface meshes.

Swaps mesh faces.

translate

Prompts for the translation offset in each of the active Cartesian coordinate directions.

bandwidth

Shows network bandwidth.

check

Performs checks of various factors that affect parallel performance.

check

Sets verbosity output of the parallel check. Higher verbosity corresponds to more detailed information.

gpgpu/

Enters the GPGPU menu

select

Selects which GPGPUs to use for AMG acceleration

show

Lists the available GPGPUs. GPGPUs selected for use are indicated by the presence of an asterisk (*).

latency

Shows network latency.

load-balance

Enters the load balancing parameters menu.

Uses physical-models load balancing?

latency

dynamic-mesh

Uses load balancing for dynamic mesh?

mesh-adaption

Uses load balancing for mesh adaption?

Enters the partition domain menu.

auto/

Sets auto partition parameters.

across-zones

Enables auto partitioning by zone or by domain.

load-vector

Sets the auto partition load vector.

method

Sets the partition method.

pre-test

Sets auto partition pre-testing optimization.

use-case-file-method

Uses partitions in a pre-partitioned case file.

combine-partition

Merges every N partitions.

merge-clusters

Calls the optimizer that attempts to decrease the number of interfaces by eliminating orphan cell

clusters. (An orphan cluster is a group of connected cells such that each member has at least one face

that is part of an interface boundary.)

method

print-active-partitions

Prints active partition information (parallel solver).

print-stored-partitions

Prints stored partition information (parallel solver).

reorder-partitions

Reorders partitions.

reorder-partitions-to-architecture

Reorders partitions to architecture.

set/

Enters the set partition parameters menu.

Allows partitions to cross zone boundaries (the default). If turned off, it will restrict partitioning to

different amounts of computation during the solution phase; for example, if the domain contains

both solid and fluid zones.

all-off

Disables all optimizations.

all-on

Enables all optimizations.

cell-function

Sets cell function.

dpm-load-balancing

all-off

all-on

Enables / disables dynamic load balancing for discrete phase model cases that use a second domain

for DPM particle tracking (that is, cases for which you have enabled the define/models/dpm/par-

allel/hybrid-2domain? text command).

face-area-as-weights

Uses face area as connection weights.

parallel/

isat-weight

Sets ISAT weight.

laplace-smoothing

Enables the Laplace smoothing option which can prevent partition boundaries from lying along

regions of high aspect ratio cells.

load-distribution

Sets the number of cells desired for each partition.This is useful, for example, when computing

on multiple machines with significantly different performance characteristics. If left unset, each

partition will contain an approximately equal number of cells. Normalized relative values may be

used for the entries.

merge

Toggles the optimizer that attempts to decrease the number of interfaces by eliminating orphan

cell clusters.

model-weighted-partition

Enables / disables model-weighted partitioning.This option works with the METIS partitioning

method, and specifies that Fluent automatically calculates the weighting based on the cell count

and the models and attributes specified as weights (using the parallel/parti-

tion/set/isat-weight text command, for example).

nfaces-as-weights

Uses number of faces as weights.

origin

Sets the ,

, and  coordinate of the origin used by those partitioning functions that require a

radial distance. By default, the origin is set to (, , ).

particle-weight

Sets DPM particle weight.

pre-test

pre-test

Enables the operation that determines the best coordinate-splitting direction.

solid-thread-weight

Uses solid thread weights.

smooth

Toggles the optimizer that attempts to minimize the number of interfaces by modifying the partition

boundaries to reduce surface area.

verbosity

Controls the amount of information that is printed out during partitioning. If set to  (the default),

a text character . is displayed during each bisection, and partition statistics are displayed once

the partitioning completes. If set to , additional information about the bisection operation is dis-

played during each bisection. If set to , partition statistics and information during each bisection

are not displayed.

vof-free-surface-weight

Sets VOF free surface weight.

smooth-partition

Calls the optimizer that attempts to minimize the number of interfaces by modifying the partition

use-stored-partitions

Uses this partitioning.

set/

Enters the set parallel parameters menu.

fast-i/o?

Uses the fast I/O option.

partition-mask

Sets partition mask.

time-out

Sets spawn time-out in seconds.

verbosity

Sets the parallel verbosity.

show-connectivity

Prints the network connectivity for the selected compute node.

Sets the maximum number of threads on each machine.

timer/

Enters the timer menu.

usage

Prints performance statistics in the console window.

reset

Adjusts domain timers.

parallel/

Chapter : plot/

circum-avg-axial

Computes iso-axial band surfaces and plots data vs. axial coordinate on them.

reset

parallel/

circum-avg-radial

Computes iso-radial band surfaces and plots data vs. radius on them.

change-fft-ref-pressure

Changes reference acoustic pressure.

display-profile-data

Plots profile data.

fft

Plots FFT of file data.

file

Plots data from an external file.

file-list

Plots data from multiple external files.

file-set/

Sets file plot parameters.

Sets the range for the  and  axes. If auto-scaling is not activated for a particular axis, you are

Sets the color of the field within the abscissa and ordinate axes.

key

Enables/disables display of curve key and sets its window title.

Sets parameters for plot lines.

Sets parameters for data markers.

labels

Sets labels for plot axes.

lines

log?

Uses log scales for one or both axes.

markers

numbers

Sets number formats for axes.

Specifies a file in which to write XY plot data.

rules

Sets parameters for display of major and minor rules.

windows/

XY plot window options. For a description of the items in this menu, see display/set/windows/xy.

flamelet-curves/

Enters the flamelet curves menu.

plot-curves

Plots of a curve property.

Writes curve to a file instead of plot.

histogram

Plots a histogram of the specified solution variable using the defined range and number of intervals.

histogram-set/

Sets histogram plot parameters. Sub-menu items are the same as file-set/ above.

plot

Plots solution on surfaces.

plot-direction

plot

Sets plot direction for XY plot.

residuals

Contains commands that allow you to select the variables for which you want to display XY plots of residual

histories in the active graphics window.

residuals-set/

Sets residual plot parameters. Sub-menu items are the same as file-set/ above.

solution

Plots solution on surfaces and/or zones. Zone and surface names can be indicated using a wildcard (*).

solution-set/

Sets solution plot parameters. Sub-menu items are the same as file-set/ above.

Sets the alignment of the xy plot label to be horizontal or axis aligned.

plot/

dpm-extended-summary

Create an extended discrete phase summary report of the discrete phase injection(s).You can choose

whether you want to save the extended report to a file or print it in the console window. For unsteady

tracking, you will be asked whether you want to include in-domain particle/tracks in the report.You will

be also prompted whether you want to select a single injection for the summary report. By default, all in-

jections are included.The output depends on whether you have enabled the report/dpm-zone-

summaries-per-injection? text command, in which case additional information is printed for escaped

particles, such as per-injection data. Note that, for unsteady particle tracking, it is necessary to enable the

report/dpm-zone-summaries-per-injection? text command before any particle parcels are

injected into the domain.

dpm-histogram/

Enters the DPM histogram menu.

compute-sample

Computes the minimum/maximum of a sample variable.

delete-sample

Deletes a sample from the loaded sample list.

list-samples

Shows all samples in a loaded sample list.

pick-sample-to-reduce

Select a sample to be reduced.

plot-sample

Plots a histogram of a loaded sample.

read-sample

Reads a sample file and adds it to the sample list.

reduce-picked-sample

Reduce a sample as specified by the data reduction parameters.This command is available only after

you selected the sample using the pick-sample-to-reduce text command.

set/

Enters the settings menu for the histogram.

Automatically computes the range of the sampling variable for histogram plots.

correlation?

Computes the correlation of the sampling variable with another variable.

cumulation-curve?

Computes a cumulative curve for the sampling variable or correlation variable when correla-

tion? is specified.

diameter-statistics?

Computes the Rosin Rammler parameters, Sauter, and other mean diameters.

histogram-mode?

Uses bars for the histogram plot or xy-style.

logarithmic?

Enables/disables the use of logarithmic scaling on the abscissa of the histogram.

maximum

Specifies the maximum value of the x-axis variable for histogram plots.

minimum

Specifies the minimum value of the x-axis variable for histogram plots.

number-of-bins

Specifies the number of bins.

percentage?

Uses percentages of bins to be computed.

variable^?

Uses the cubic of the cumulation variable during computation of the cumulative curve.

weighting?

Uses weighting with additional variables when sorting data into samples.

write-sample

Writes a histogram of a loaded sample into a file.

setup-reduction/

Enters the settings menu for the sample data reduction.This command is available only after you se-

lected the sample using the pick-sample-to-reduce text command.

all-variables-number-of-bins

Sets the number of bins to be used for all variables in the data reduction.

list-settings

Prints all current sample data reduction settings for all variables in the selected sample in the

console.

Enables/disables the logarithmic scaling for a selected variable.

make-steady-from-unsteady-file?

Enables/disables the unsteady sample reduction into a steady-state injection file.This command

is available only for sample files from unsteady particle tracking.

maximum

Sets the maximum value of the range to be considered for a specific variable.

report/

minimum

Sets the minimum value of the range to be considered for a specific variable.

Sets the number of bins for a specific variable.

reset-min-and-max

Resets the specified maximum and minimum values for a specific variable.

use-weighting?

Enables/disables the use of weighting in the data averaging in each bin.

weighting-variable

Sets the weighting variable for the data averaging in each bin.

dpm-sample

Samples trajectories at boundaries and lines/planes.

dpm-sample-output-udf

Allows you to hook a previously loaded DEFINE_DPM_OUTPUT UDF for file format specification for

sampling of trajectories and VOF-to-DPM lump conversion transcripts.

dpm-sample-sort-file?

Enables/disables writing of sorted DPM sample files.

dpm-summary

Prints discrete phase summary report.

dpm-zone-summaries-per-injection?

Enables/disables calculation of the escaped mass per injection. Note that for unsteady particle tracking, if

you want to report the mass of escaped particles per injection, this text command must be enabled before

any particles are injected into the domain.

element-mass-flow

Prints list of element flow rate at inlets and outlets.This reports the mass flow rates of all chemical elements

(in kg/s) flowing through the simulation boundaries.

fluxes/

Enters the fluxes menu.

film-heat-transfer

Prints wall film heat transfer rate at boundaries.This text command is only available when you enable

the Eulerian wall film model.

film-mass-flow

Prints wall film mass flow rate at boundaries.This text command is only available when you enable

heat-transfer

Prints heat transfer rate at boundaries.

heat-transfer-sensible

Prints the sensible heat transfer rate at the boundaries.

mass-flow

Prints mass flow rate at inlets and outlets.

rad-heat-trans

Prints radiation heat transfer rate at boundaries.

forces/

Enters the forces menu.

pressure-center

Prints the center of pressure on wall zones.

wall-forces

Computes the forces along the specified force vector for all wall zones.

wall-moments

Computes the moments about the specified moment center for all wall zones.

computed-heat-rejection

Prints total heat rejection.

inlet-temperature

Prints inlet temperature.

outlet-temperature

Prints outlet temperature.

mass-flow-rate

Prints mass flow rate.

specific-heat

Prints fluid’s specific heat.

mphase-summary

Prints summary report for a multiphase case setup.

particle-summary

Prints summary report for all current particles.

path-line-summary

Prints pathline summary report.

print-histogram

Prints a histogram of a scalar quantity.

projected-surface-area

Computes the area of the projection of selected surfaces along the ,

, or  axis.

reference-values/

Enters the reference value menu.

report/

area

Sets reference area for normalization.

compute/

Computes reference values from zone boundary conditions.

density

Sets reference density for normalization.

depth

Sets reference depth for volume calculation.

enthalpy

Sets reference enthalpy for enthalpy damping and normalization.

length

Sets reference length for normalization.

list

Lists current reference values.

pressure

Sets reference pressure for normalization.

Sets reference temperature for normalization.

velocity

Sets reference velocity for normalization.

viscosity

Sets reference viscosity for normalization.

zone

Sets reference zone.

species-mass-flow

Prints list of species mass flow rate at inlets and outlets.This reports the mass flow rates of all species (in

kg/s) flowing through the simulation boundaries.

summary

Prints the current settings for physical models, boundary conditions, material properties, and solution

surface-integrals/

Enters the surface integral menu.

area

Prints the area of the selected surfaces.

area-weighted-average

Prints area-weighted average of the specified quantity over the selected surfaces.

facet-avg

area

facet-avg

Prints the facet average of the specified quantity over the selected surfaces.

facet-max

Prints the maximum of the specified quantity over facet centroids of the selected surfaces.

facet-min

Prints the minimum of the specified quantity over facet centroids of the selected surfaces.

flow-rate

Prints the flow rate of the specified quantity over the selected surfaces.

integral

Prints the integral of the specified quantity over the selected surfaces.You can include a wildcard (*)

within the surface names.

Prints the mass flow rate through the selected surfaces.

mass-weighted-avg

Prints the mass-averaged quantity over the selected surfaces.

standard-deviation

Prints the standard deviation of the scalar at the facet centroids of the surface.

sum

Prints sum of scalar at facet centroids of the surfaces.

uniformity-index-area-weighted

Prints the area-weighted uniformity index of the specified quantity over the selected surfaces.

uniformity-index-mass-weighted

Prints the mass-weighted uniformity index of the specified quantity over the selected surfaces.

vector-based-flux

Prints the vector-based flux of the specified quantity over the selected surfaces.

vector-flux

Prints the vector flux over the selected surfaces.

vector-weighted-average

Prints the vector-averaged quantity over the selected surfaces.

vertex-avg

Prints the vertex average of the specified quantity over the selected surfaces.

vertex-max

Prints the maximum of the specified quantity over vertices of the selected surfaces.

vertex-min

Prints the minimum of the specified quantity over vertices of the selected surfaces.

volume-flow-rate

Prints the volume flow rate through the selected surfaces.

system/

Enters the system menu.

report/

gpgpu-stats

Prints information about installed general purpose graphical processing units.

proc-stats

Prints ANSYS Fluent process information.This is used to report the memory usage of each of the ANSYS

Fluent processes.

sys-stats

System information.This is used to report the CPU configuration of the machines where ANSYS Fluent

processes have been spawned.

time-stats

Timer information.This is used to report CPU timings for user and kernel processes and detailed solver

timings.

uds-flow

Prints list of user-defined scalar flow rate at boundaries.

volume-integrals/

Enters the volume integral menu.

mass

Prints total mass of a phase within a selected cell zone.

mass-avg

Prints mass-average of scalar over cell zones.

mass-integral

Prints mass-weighted integral of scalar over cell zones.

maximum

Prints maximum of scalar over all cell zones.

minimum

Prints minimum of scalar over all cell zones.

sum

Prints sum of scalar over all cell zones.

twopisum

Prints sum of scalar over all cell zones multiplied by 2π.

volume

Prints total volume of specified cell zones.

volume-avg

Prints volume-weighted average of scalar over cell zones.

volume-integral

Prints integral of scalar over cell zones.

Chapter : server/

start-client

Start the ANSYS Fluent remote visualization client.

start-server

Starts the server for the ANSYS Fluent remote visualization client.

print-connected-clients

Prints the name of the connected client and its IP address to the console.

print-server-address

Prints the host address and port number of the server to the console.

shutdown-server

Shuts-down the server and disconnects the connected client.

write-or-reset-server-info

Allows you to create a new server_info.txt file (with any name you specify), which resets the password

for connecting to this server session. It does not restart the server.

Chapter : solve/

animate/

Enters the animation menu.

define/

Changes animation monitor attributes.

objects/

Enters the object manipulation menu.

Clears solution animation object history.

copy

Copies solution animation object.

create

Creates new solution animation object.

delete

Deletes solution animation object.

edit

Edits solution animation object.

playback/

delete

play

read

Reads new animation from file or already defined animations.

write

cell-register-operations/

Enters the cell register operations menu.

add

Creates a new cell register operation.

delete

Deletes a cell register operation.

edit

Edits an existing cell register operation.

list

Lists the currently defined cell register operations.

Lists the properties of a report register operation.

edit

list

add

coarsen

delete

display

edit

list

refine

convergence-conditions/

Enters the convergence conditions menu.

condition

Specifies whether the solution is considered converged when all of the conditions are met or when

one of the conditions is met.

solve/

conv-reports/

Enters the convergence reports menu.

add

Creates a new convergence condition.

delete

Deletes a convergence condition.

edit

Edits a convergence condition.

list

Lists all of the report definition-based convergence conditions.

Lists the properties of the specified convergence condition.

frequency

Specifies how often convergence checks are performed.

dpm-update

Updates discrete phase source terms.

dual-time-iterate

Performs unsteady iterations for a specified number of time steps.

Enters the execute commands menu.

add-edit

Adds or edits execute commands.

disable

Disables an execute command.

enable

Enables an execute command.

initialize/

Enters the flow initialization menu.

compute-defaults/

Enters the compute default values menu.

all-zones

Initializes the flow field with the default values.

zone

all-zones

zone

You can select the type of zone from which you want to compute these values.The types of zones

available are:

axis

degassing

fan

fluid

interface

interior

network

network-end

outflow

periodic

radiator

shadow

solid

symmetry

wall

dpm-reset

Resets discrete phase source terms to zero.

solve/

fmg-initialization

Initializes using the full-multigrid initialization (FMG).

hyb-initialization

Initializes using the hybrid initialization method.

init-acoustics-options

Specifies the number of timesteps for ramping of sound sources and re-initializes the acoustics wave

equation solution. For the initialized acoustics solution, Fluent reports the current state of the sound

sources ramping.

init-flow-statistics

Initializes unsteady statistics.

initialize-flow

Initializes the flow field with the current default values.

init-turb-vel-fluctuations

Initializes instantaneous velocity field out of steady state RANS results, for use before enabling a scale

resolving simulation such as LES.

list-defaults

Lists default values.

open-channel-auto-init

Opens channel automatic initialization.

reference-frame

Sets reference frame to absolute or relative.

set-defaults/

Sets default initial values.

set-fmg-initialization/

Enters the set full-multigrid for initialization menu. Initial values for each variable can be set within this

menu.

set-hyb-initialization/

Enters the hybrid initialization menu.

general-settings

Enters the general settings menu.

turbulence-settings

Enters the turbulence settings menu.

species-settings

Enters the species-settings menu.

show-iterations-sampled

Displays the number of iterations covered by the data sampled for steady statistics.

show-time-sampled

Displays the amount of simulated time covered by the data sampled for unsteady statistics.

vof-patch-smooth-options/

Enters the vof patch/smooth options menu.

execute-smoothing

Performs volumetric smoothing for volume fraction.

set-options

Sets options for patching and smoothing volume fraction.

iterate

Performs a specified number of iterations.

Note

This option is still available during transient simulations, since it can be used to add more

iterations to the same time step after interrupting iterations within a time step.

mesh-motion

Performs mesh motion.

monitors/

Sets solution monitors.

residual/

Enters the residual monitors menu.

check-convergence?

Chooses which currently monitored residuals should be checked for convergence.

Sets convergence criteria for residuals that are currently being both monitored and checked.

criterion-type

Sets convergence criterion type.

monitor?

Chooses which residuals to monitor as printed and/or plotted output.

n-display

Sets the number of most recent residuals to display in plots.

n-maximize-norms

monitor?

n-display

Sets the number of iterations through which normalization factors will be maximized.

normalization-factors

Sets normalization factors for currently monitored residuals (if normalize? is set to yes).

normalize?

Chooses whether to normalize residuals in printed and plotted output.

solve/

n-save

Sets number of residuals to be saved with data. History is automatically compacted when buffer

becomes full.

plot?

Chooses whether residuals will be plotted during iteration.

print?

Chooses whether residuals will be printed during iteration.

relative-conv-criteria

Sets relative convergence criteria for residuals that are currently being both monitored and checked.

re-normalize

Re-normalize residuals by maximum values.

reset?

Chooses whether to delete the residual history and reset iteration counter to .

scale-by-coefficient?

Chooses whether to scale residuals by coefficient sum in printed and plotted output.

window

Specifies window in which residuals will be plotted during iteration.

patch

Patches a value for a flow variable in the domain.

report-definitions/

Enters the report definitions menu.

add

Creates a report definition.

copy

Creates a copy of a report definition.

delete

Deletes a report definition.

edit

Edits a report definition.

list

Lists all defined report definitions.

Lists the properties of a report definition.

rename

Renames a report definition.

report-files/

Enters the report files menu.

add

Creates a report file.

clear-data

Clears the data associated with a report file.

delete

Deletes a report file.

edit

Edits a report file.

list

add

delete

edit

list

Lists all defined report files.

Lists the properties of a report file.

report-plots/

Enters the report plots menu.

add

Creates a report plot.

axes

Defines the axes for a report plot.

Clears the data associated with a report plot.

curves

Defines the curves for a report plot.

delete

Deletes a report plot.

edit

Edits a report plot.

list

Lists all defined report plots.

Lists the properties of a report plot.

plot

Plots the specified report plot.

rombuilder/

Enters the rombuilder menu.

enable?

Enables/disables the reduced order model.

solve/

evaluate

Allows you to enter values between the allowed ranges for the existing variables and zones that are

part of the loaded ROM and have the results computed (when a ROMZ file is loaded into Fluent in

Workbench).

select-variables-and-zones

Select the variables and locations that you want included in the reduced order model.

set/

Enters the set solution parameters menu.

accelerated-non-iterative-time-marching

Enables a modified NITA scheme and other setting changes that can speed up the simulation.This

option is only available with the Large Eddy Simulation (LES) turbulence model, and is intended for

unreacting flow simulations that use a constant-density fluid.

acoustics-wave-equation-controls/

Enters the menu to specify parameters of the acoustics wave equation solver.

expert/

Enters the menu to specify the expert parameters.

explicit-relaxation-factor

Specifies the explicit relaxation factor. Should be used only with bad meshes, when iterations

do not converge.

under-relaxation-factor

Specifies the implicit under-relaxation factor. Should be used only with bad meshes, when the

AMG linear solver does not converge.

max-iterations-per-timestep

Specifies the maximum number if iterations, which will be performed by the acoustics wave

equation solver in one timestep.

relative-convergence-criterion

Specifies the iterations convergence criterion in terms of the residual norm drop.

amg-options/

Enters the AMG options menu

aggressive-amg-coarsening?

Enables / disables the use of a version of the AMG solver that is optimized for high coarsening

rates.This option is recommended if the AMG solver diverges with the default settings.

amg-gpgpu-options/

Enters the AMG GPGPU options menu, which contains commands to enable / disable GPGPU ac-

celeration and set solver type and options for individual coupled and scalar equations.

conservative-amg-coarsening?

Enables / disables the use of conservative coarsening techniques for scalar and/or coupled equations

that can improve parallel performance and/or convergence for some difficult cases.

laplace-coarsening?

Enables / disables Laplace coarsening for scalar and/or coupled equations.

bc-pressure-extrapolations

Sets pressure extrapolations schemes on boundaries.

If you are using the density-based solver, you will be asked the following questions:

extrapolate total quantities on pressure-outlet boundaries?

The default is [no]. If you enter yes, and the flow leaving the pressure outlet is subsonic, then

the total pressure and total temperature from the domain’s interior are extrapolated to the

boundary and used with the imposed static pressure to determine the full thermodynamic state

at the boundary.

extrapolate pressure on pressure-inlet boundary?

The default is [no]. If you enter yes, then for cases with very low Mach number flow in the single-

precision density-based solver, you can improve convergence by using pressure extrapolation in-

stead of the default velocity extrapolation scheme.

pressure on pressure-outlet b.c. is obtained via an advection splitting

method?

The default is [yes]. If you choose the default, this means that the pressure-outlet boundary

condition implementation in the density-based solver has an absorption behavior, as described

in Calculation Procedure at Pressure Outlet Boundaries of the User’s Guide.To revert to pre-ANSYS

Fluent . boundary condition implementations, where the pressure on the faces of a pressure-

outlet boundary is fixed to the specified value while the flow is subsonic, enter no.

Important

The absorption behavior of the pressure-outlet boundary condition should not

be confused with rigorous non-reflecting boundary condition implementation,

described in Boundary Acoustic Wave Models of the User’s Guide.

If you are using the pressure-based solver, you will be asked the following questions:

extrapolate pressure on flow inlets?

The default is [yes].

extrapolate pressure on all boundaries?

The default is [no].

extrapolate velocity on out-flow boundaries?

cfl-based-time-stepping

Allows you to specify that an adaptive time stepping method is used in which the time step gets

modified by ANSYS Fluent as the calculation proceeds such that the Courant–Friedrichs–Lewy (CFL)

condition is satisfied, using the specified Courant number.

convergence-acceleration-for-stretched-meshes/

Enables convergence acceleration for stretched meshes to improve the convergence of the implicit

density based solver on meshes with high cell stretching.

correction-tolerance/

Enters the correction tolerance menu.

solve/

coupled-vof-expert

Sets coupled vof expert controls.You will be prompted with the following questions:

Use linearized buoyancy force?

Provides the implicit linearization of buoyancy force.

Use blended treatment for buoyancy force?

Will turn off buoyancy linearization in certain unstable conditions.

Use false time step linearization?

Provides additional stability for buoyancy driven flows in the steady-state pseudo-transient mode

by increasing the diagonal dominance using false time step size.

Use smoothed density for pseudo-transient method?

Smooths the cell density near the interface, therefore avoiding unphysical acceleration of lighter

phase in the vicinity of interface.This option is only available for steady-state pseudo-transient

method.

Note

There is an additional entry for the number of density smoothings (default ), which

can be increased in case of very large unphysical velocities across the interface.

courant-number

Sets the fine-grid Courant number (time step factor).This command is available only for the coupled

solvers.

data-sampling

solvers.

Enables data sampling for steady or unsteady flow statistics.

disable-reconstruction?

Completely disables reconstruction, resulting in totally first-order accuracy.

discretization-scheme/

Enters the discretization scheme menu.This allows you to select the discretization scheme for the

convection terms in the solution equations.The following text commands can make a selection from

a subset of the models in the following table:

Model

Index

QUICK

Third-Order MUSCL

Bounded Central

Differencing

CICSAM

Standard

Model

Index

Linear

Second Order

Body Force Weighted

PRESTO!

BGM

amg-c

Selects the discretization scheme for the flow equations.

epsilon

Selects the discretization scheme for the turbulent dissipation rate.

k

Selects the discretization scheme for the turbulent kinetic energy.

mom

Selects the discretization scheme for momentum.

mp

Selects which convective discretization scheme for volume fraction is to be used.

pressure

Selects the discretization scheme for pressure.

Selects the discretization scheme for energy.

divergence-prevention/

Enters the divergence prevention menu.This menu is only available for the density-based solver.

enable?

Enables a divergence prevention option so that Fluent applies under-relaxation to the variables

in select cells where the temperature and/or pressure values are approaching the minimum and/or

maximum limits.

duration-specification-method

Sets the method by which you will specify the duration of the calculation.The duration can be defined

by the total time, the total number of time steps, the incremental time, or the number of incremental

time steps. In this context, "total" indicates that Fluent will consider the amount of time / steps that

have already been solved and stop appropriately, whereas "incremental" indicates that the solution

will proceed for a specified amount of time / steps regardless of what has previously been calculated.

This text command is only available when the time stepping is adaptive or based on a user-defined

function.

enable-output-dp-dt?

Controls whether the output field variable dp-dt will be available for transient simulation postprocessing.

If you select no, pressure fields at the previous time steps will not be stored in memory which reduces

memory usage.

solve/

equation-ordering

Sets the order in which the model equations are solved, which can affect the convergence speed when

you are using the pressure-based solver.The standard method is enabled by default and corresponds

to the ordering shown in Figure . : Overview of the Iterative Time Advancement Solution Method

For the Segregate Solver and Figure . : Overview of the Non-Iterative Time Advancement Solution

Method in the Theory Guide; alternatively, you can select the optimized-for-volumetric-ex-

pansion method, which is recommended for flows in which the density is strongly dependent on

thermal effects, chemical composition, and so on (such as combustion simulations).This text command

is not available for steady simulations and/or when a multiphase model is enabled.

equations/

Selects the equations to be solved.

error-based-time-stepping

modified by ANSYS Fluent  based on the specified truncation error tolerance.

expert

Sets expert options.

extrapolate-eqn-vars/

Enters the extrapolation menu.

extrapolate-vars?

Applies a predictor algorithm for computing initial conditions at time step n+.The predictor algorithm

is a computation that sets a better initial condition for the time step.

fast-transient-settings/

Enters the fast transient settings menu.This menu is only available for transient cases that use the

rk2

Allows you to enable the use of a two-stage Runge-Kutta scheme for time integration, or revert to

the default multi-stage Runge-Kutta scheme.This text command is only available for transient

cases that use the density-based explicit formulation.

fixed-periodic

Allows you to specify that a fixed time stepping method is used in which a specified period or frequency

is the basis for determining the time step size and number of time steps.

fixed-user-specified

Allows you to specify that a fixed time stepping method is used in which you directly specify the time

step size and number of time steps.

flow-warnings?

Specifies whether or not to print warning messages when reversed flow occurs at inlets and outlets,

and when mass-flow inlets develop supersonic regions. By default, flow warnings are printed.

flux-type

Sets the flux type.

gradient-scheme

Sets gradient options.

heterogeneous-stiff-chemistry

Sets the heterogeneous stiff-chemistry solver.

high-order-term-relaxation/

flux-type

Enters the High Order Term Relaxation menu.

enable?

Enables/disables High Order Term Relaxation.

options/

High Order Term Relaxation Options.

Sets the relaxation factor.

variables/

Selects the variables.

incremental-time

Sets the amount of incremental (that is, additional) time to run the simulation, regardless of how much

time has already been run in previous calculations.This text command is only available when the

solve/set/duration-specification-method is set to .

limiter-warnings?

Specifies whether or not to print warning messages when quantities are being limited. By default,

limiter warnings are printed.

limits

Sets solver limits for various solution variables, in order to improve the stability of the solution.

lock-solid-temperature?

Specifies whether you want to lock (or “freeze”) the temperature values for all the cells in solid zones

(including those to which you have a hooked an energy source through a UDF) and in walls that have

shell conduction enabled, so that the values do not change during further solver iterations.

mp-mfluid-aniso-drag

Sets anisotropic drag parameters for the Eulerian multiphase model.

mp-reference-density

Sets the reference density option for the Eulerian multiphase model.The following options are available:

VOF Equation Discretization Option

Index

reference density for a particular phase in a cell is

treated as the volume averaged density of that phase

in the whole domain

mass conservative

treated as the density of that phase in that cell

reference density for any phase in a cell is treated as

the mixture density of that phase in that cell

volume conservative

solve/

max-corrections/

Enters the set max-corrections menu.

max-flow-time

Sets the maximum flow time.

max-iterations-per-time-step

Sets the number of time steps for a transient simulation.

Note

This option is available when automatic initialization and case modification is enabled.

multi-grid-amg

Sets the parameters that govern the algebraic multigrid procedure.

multi-grid-controls/

Sets multigrid parameters and termination criteria.

multi-grid-fas

Sets the parameters that control the FAS multigrid solver.This command appears only when the explicit

coupled solver is used.

multi-stage

Sets the multi-stage coefficients and the dissipation and viscous evaluation stages.This command

appears only when the explicit coupled solver is used.

multiphase-numerics

Sets multiphase numerics options.

boiling-parameters/

Enters the menu for the multiphase boiling model parameters.

liquid-vof-factor

When enabled, considers liquid volume fraction effects by multiplying the heat transfer coeffi-

cients by the local liquid volume fraction.

thin-film

When enabled, includes multiphase boiling thin film effects using Equation . in the Fluent

compressible-flow/

Enters the compressible multiphase flow numerics menu.

alternate-bc-formulation

Enables an alternative formulation for compressible phases at an inlet boundary.This formulation

calculates static temperature and pressure using an iterative method based on fundamental

thermodynamic relations.

enhanced-numerics

Enables an enhanced numerical treatment that provides better stability at startup and during

calculation of compressible flows.

heat-mass-transfer/

Enters the menu for the multiphase heat mass transfer parameters.

alternative-energy-treatment?

Enables the alternative treatment of the energy sources. For more information, see Including

Mass Transfer Effects in the Fluent User's Guide.

area-density/

Enters the menu for the area density.

ia-grad-sym?

Enables/disables the interfacial area density Gradient-Symmetric model. For more inform-

ation about this model, see Algebraic Models in the Fluent Theory Guide.

vof-min-seeding

Sets the minimum volume fraction for the area density and cavitation.This may be useful,

for example, in cases when a species mass transfer model (such as the Symmetric model

or Particle model) do not consider evaporation or condensation if the volume fraction of

one of the phases is zero.The seeding allows for a phase change to occur in the fluid flow.

The default value is 1e-.

boiling/

Enters the menu for the advanced boiling options for the semi-mechanistic boiling model.

heat-flux-relaxation-factor

Sets the under-relaxation factor for boiling heat flux. See Solution Strategies for the Semi-

Mechanistic Boiling Model in the Fluent User's Guide for details.

show-expert-options?

Exposes the expert options for the semi-mechanistic boiling model. For more information

about these options, see Expert Options for the Semi-Mechanistic Boiling Model in the

Enters the cavitation heat mass transfer menu.

min-vapor-pressure

Sets the minimum vapor pressure limit for the cavitation mass-transfer model.The default

value is  Pa.

max-vapor-pressure-ratio

Sets the maximum limit on the vapor pressure after the turbulence and thermal correction.

The default value is five times the vapor pressure, with consideration of turbulent and

thermal effects for each cell and phase.

schnerr-cond-coeff

Sets the condensation coefficient for the Schnerr-Sauer model (

in the Fluent Theory Guide).The default and recommended value of ..

schnerr-evap-coeff

Sets the evaporation coefficient for the Schnerr-Sauer model (

the Fluent Theory Guide).The default and recommended value of .

solve/

turbulent-diffusion

enables/disables the turbulent diffusion treatment for a cavitating turbulent flow. See Mass

Transfer Mechanisms in the Fluent User's Guide for details.

nita-controls/

Enters the NITA controls menu.

face-pressure-options

Sets face pressure options for the pressure calculation.When prompted with enable body-

force-weighted for face pressure calculation?, enter yes to select Body

Force Weighted and no to select Second Order as a face pressure interpolation method. See

Controlling NITA Solution Options via the Text Interface in the Fluent User's Guide for details.

porous-media/

Enters the porous media numerics menu.

relative-permeability

Allows you to fix the saturation (volume fraction) of the phase at its user-specified residual

saturation value.

viscous-flow

Enters the viscous multiphase flow numerics menu.

viscosity-averaging

Forces harmonic averaging of cell viscosities to calculate face viscosity used in momentum

equation.This can improve convergence for highly viscous flow applications (the VOF model

only).

multiphase-specific-time-stepping

modified by ANSYS Fluent  based on the convective time scale (global Courant number): the time-step-

size calculation depends on the mesh density and velocity in interfacial cells.This method is available

for all multiphase models using the implicit or explicit volume fraction formulation, except for the wet

steam model.

nb-gradient-boundary-option?

Switches between the modified treatment of node-based gradients at boundary cells and the legacy

treatment (R14.. and earlier).

nita-expert-controls/

Enters the NITA expert control menu.

hybrid-nita-settings

Enables and sets hybrid NITA options. For more details, see User Inputs in the Fluent User's Guide.

set-verbosity

Setting this to , enables the verbosity for NITA diagnostics.The default value of  disables verbosity

output for NITA diagnostics.

skewness-neighbor-coupling

Enables/disables coupling of the neighbor and skewness corrections.

number-of-iterations

Sets the number of iterations for a steady-state simulation without starting the calculation.

number-of-time-steps

Sets the number of time steps for a transient simulation without starting the calculation.

numerical-beach-control

Sets damping function in flow direction.This command appears only when the VOF model is enabled.

Select the damping function to be used:

Damping Function

Index

Linear

Quadratic

Cubic

Cosine

numerics

Sets numerics options.

open-channel-controls

For flows that do not transition from sub-critical to super-critical, or vice-versa, you can speed-up the

solution calculation by updating the frequency of Froude number during run time.

open-channel-wave-options/

Sets buffer layer height, verbosity, and open channel wave theory formulation.

set-buffer-layer-ht

Sets the buffer layer height.

Sets the open channel wave verbosity.

stokes-wave-variants

Specifies which open channel wave theory formulation Fluent uses.

overset/

Specifies overset meshing solver options.

high-order-pressure?

Uses the pressure gradient of the donor cell in the interpolation of pressure for its receptor cell.

Selects the interpolation method for overset interfaces. Note that the least squares method is re-

commended for sliding mesh cases.

orphan-cell-treatment?

Enables/disables a numerical treatment that attempts to assign reasonable data values to orphan

cells.

p-v-controls

Sets pressure-velocity controls.

p-v-coupling

Selects which pressure-velocity coupling model is to be used. Four models are available:

solve/

Model

Index

SIMPLE

SIMPLEC

PISO

Coupled

phase-based-vof-discretization

Sets phase based slope limiter for VOF compressive scheme.

poor-mesh-numerics/

solve/

Model

Index

SIMPLE

SIMPLEC

PISO

Coupled

Enters the poor mesh numerics menu.

cell-quality-based?

Enables/disables poor mesh numerics on cells with low quality.

enable?

Solution correction on meshes of low quality.

print-poor-elements-count

Prints out a listing of the poor cells for each criterion (default, cell quality, and user-defined).

reset-poor-elements?

Resets the list of poor cells included based on quality criteria or user-defined registers.

set-quality-threshold

Sets the threshold for quality-based inclusion in the poor mesh numerics.The threshold value is

applied to cell orthogonality and the complement of cell skewness.

user-defined-on-register

Includes a register for the poor mesh numerics or not.

predict-next-time?

Applies a predictor algorithm for computing the next time step.The predictor algorithm is a computation

that sets a better initial condition for the time step. It uses the rate of change between the prediction

and the correction as an indicator for whether the next time step should be larger, smaller, or the same

as the current one.

previous-defaults/

Provides text commands that allow you to undo enhancements to the default solver behavior.

undo-2019r1-default-changes?

Allows you to undo enhancements introduced in version  R1 of ANSYS Fluent, including:

Maintaining positivity for turbulence variables.These enhancements affect the solution when

using an overset interface with the default least squares interpolation method, and may affect

convergence when using an

based turbulence model or a second-order advection scheme

for the turbulence equations. On occasion, these enhancements may have a small adverse effect

on performance.

Using the coupled pseudo-transient solver as a default solver for steady-state, single-phase

problems (except for cases that use the battery, fuel cells, melting, or solidification models). If

you choose to undo these enhancements, the pressure-velocity coupling scheme will revert to

its previous setting.

Using a more aggressive pseudo time step size for the automatic pseudo time scale method.

This enhancement affects the solution when using the coupled pseudo-transient solver and may

improve convergence in some cases.

Allows you to undo enhancements introduced in version  R3 of ANSYS Fluent, including:

Using a formulation for the Rhie-Chow face flux interpolation for single-phase simulations

that includes a velocity reconstruction designed to handle non-uniform meshes. For such

meshes, this formulation gives more accurate results and prevent non-physical reflections

of error waves. Note that this formulation may require you to use a smaller flow Courant

number or pseudo time step size when you are using the pressure-based coupled solver.

Using a discretization for poor mesh numerics that enhances robustness for meshes with

wall boundary layer resolution (for example, y+=). This discretization is especially effective

at wall surfaces that have high curvature and/or high aspect ratios of the near-wall cells.

It is primarily intended to prevent divergence, though it may also improve the solution

accuracy.

accuracy.

Allows you to undo enhancements introduced in version . of ANSYS Fluent, including the

treatment of symmetry boundary conditions and the treatment of walls with the specified shear

condition, as well as an early protection scheme for the linear solver.

pseudo-relaxation-factor/

Enters the pseudo relaxation factor menu.

pseudo-transient

Sets the pseudo transient formulation.

pseudo-transient-expert/

Enters the pseudo transient expert usage control menu.

reactions?

Enables the species reaction sources and sets relaxation factor.

relaxation-factor/

Enters the relaxation-factor menu.

relaxation-method

Sets the solver relaxation method.

reporting-interval

Sets the number of iterations for which convergence monitors are reported.The default is  (after

every iteration).

residual-smoothing

Sets the implicit residual smoothing parameters.This command is available only for the explicit coupled

solver.

residual-tolerance/

Enters the residual tolerance menu.

solve/

residual-verbosity

Sets the amount of residual information to be printed. A value of  (the default) prints residuals at the

end of each fine grid iteration. A value of  prints residuals after every stage of the fine grid iteration.

A value of  prints residuals after every stage on every grid level.

rotating-mesh-flow-predictor?

Enables / disables an option that allows for better prediction of the flow field in rotating fluid zones

at every time step, in order to speed up the calculation.This text command is only available for transient

simulations.

second-order-time-options

Enables / disables the variable time step size formulation for second-order implicit transient formulations.

If you disable the variable time step size formulation, note that any change in the time step size will

introduce an error proportional to the change in the time step size ratio.

set-all-species-together

Sets all species discretizations and URFs together.

set-controls-to-default

Sets controls to default values.

set-solution-methods-to-default

Sets the solution methods to the default settings.

set-solution-steering

Sets solution steering parameters.

slope-limiter-set/

Selects a new Fluent solver slope limiter.

solid-time-step-size

Allows you to specify that the time step size used for solid zones is independent from that used for

fluid zones.This text command is only available when both a solid zone exists and energy is enabled.

solution-status

Allows you to open the Simulation Status dialog box, which reports details about the simulation.

solution-steering

Enables solution steering for the density-based solver.

stiff-chemistry

Sets solver options for stiff chemistry solutions.

surface-tension

Sets surface-tension calculation options.

time-step-size

Sets the magnitude of the (physical) time step

.This text command is only available when the

solve/set/fixed-user-specified text command is set to yes.

total-number-of-time-steps

Sets the total number of time steps that the simulation will run (which includes any time steps that

have already been run in previous calculations).This text command is only available when the

total-time

Sets the total amount of time that the simulation will be run (which includes any time that has already

been run in previous calculations).This text command is only available when the solve/set/dura-

tion-specification-method is set to .

udf-based-time-stepping

Allows you to specify that the time step size is defined by a user-defined function (UDF) that uses the

DEFINE_DELTAT macro.

under-relaxation/

Enters the under-relaxation menu, which allows you to set the under-relaxation factor for each equation

that is being solved in a segregated manner.

undo-timestep

When enabled, if the truncation error within a time step exceeds the specified tolerance Fluent will

automatically undo the current calculation and make another attempt with the time step reduced by

/.This will be attempted up to  times after which Fluent will accept the result and proceed to the

next time step.

vof-explicit-controls

Sets the sub time step calculation method for VOF calculations.

vof-numerics

Sets VOF numeric options.

warped-face-gradient-correction/

Enters the warped-face gradient correction menu.

enable?

Enables/disables gradient enhancement computations and specifies whether Fluent uses fast or

memory saving mode.

update-physical-time

Advances the unsteady solution to the next physical time level. Using this command in conjunction with

the iterate command allows you to manually advance the solution in time (rather than doing it auto-

matically with the dual-time-iterate command).

solve/

Chapter : surface/

circle-slice

Extracts a circular slice.

delete-surface

Removes a defined data surface.

edit-surface

solve/

Allows you to edit any of the listed available surfaces.

imprint-surface

Enters the list of surfaces to imprint from and the name of the new imprinted surface.

iso-clip

Clips a data surface (surface, curve, or point) between two isovalues.

iso-surface

Extracts an iso-surface (surface, curve, or point) from the current data field.

line-slice

Extracts a linear slice in 2D, given the normal to the line and a distance from the origin.

line-surface

Defines a “line" surface by specifying the two endpoint coordinates.

list-surfaces

Displays the ID and name, and the number of point, curve, and surface facets of the current surfaces.

mouse-line

Extracts a line surface that you define by using the mouse to select the endpoints.

mouse-plane

Extracts a planar surface defined by selecting three points with the mouse.

mouse-rake

Extracts a “rake" surface that you define by using the mouse to select the endpoints.

multiple-zone-surfaces

Creates multiple data surfaces at one time. Accepts zone names, lists of zone ID’s, and wildcards.

partition-surface

Defines a data surface consisting of mesh faces on the partition boundary.

plane

Creates a plane given  points bounded by the domain.

plane-bounded

Creates a bounded surface.

plane-point-n-normal

Creates a plane from a point and normal.

plane-slice

Extracts a planar slice.

plane-surf-aligned

Creates a plane aligned to a surface.

plane-view-plane-align

Creates a plane aligned to a view-plane.

point-array

Extracts a rectangular array of data points.

point-surface

Defines a “point" surface by specifying the coordinates.

quadric-slice

Extracts a quadric slice.

rake-surface

Extracts a “rake" surface, given the coordinates of the endpoints.

rename-surface

Renames a defined data surface.

reset-zone-surfaces

Recreates missing surface zones by resetting the case surface list.

sphere-slice

Extracts a spherical slice.

structural-point-surface

Defines a structural “point" surface by specifying the coordinates.

Extracts all cells intersected by a data surface.

transform-surface

Transforms surface.

zone-surface

Creates a surface of a designated zone and gives it a specified name.

surface/

Chapter : switch-to-meshing-mode

switch-to-meshing-mode

Switches from the solution mode to the meshing mode.This text command is only available if you have

not yet read a mesh or a case file.

Chapter : turbo/

2d-contours

Displays 2D contours.

avg-contours

Displays average contours.

compute-report

Computes turbomachinery quantities.

current-topology

Sets the current turbo topology for global use.

write-report

Writes the turbo report to file.

xy-plot-avg

Displays average XY plots.

Chapter : views/

Scales and centers the current scene without changing its orientation.

camera/

Enters the camera menu to modify the current viewing parameters.

Adjusts the camera position and target.

field

Sets the field of view (width and height).

Adjusts the camera position without modifying the target.

Adjusts the camera target without modifying the position.

position

Sets the camera position.

position

Toggles between perspective and orthographic views.

Adjusts the camera up-vector.

target

Sets the point to be the center of the camera view.

up-vector

Sets the camera up-vector.

Adjusts the camera’s field of view.This operation is similar to dollying the camera in or out of the scene.

Dollying causes objects in front to move past you. Zooming changes the perspective effect in the scene

(and can be disconcerting).

Resets view to front and center.

Removes a view from the list.

last-view

Returns to the camera position before the last manipulation.

Lists predefined and saved views.

Reads views from a view file.

Uses a saved view.

save-view

Saves the current view to the view list.

Writes selected views to a view file.

views/

Chapter : battery-model/

This chapter has the following sections:

.. Single-Potential Empirical Battery Model

.. Dual-Potential MSMD and Circuit Network Battery Models

Once the battery module is loaded, you can access the text user interface through the Console Window

under battery-model. A listing of the various text commands is as follows:

battery-model/

Enters the battery model menu

activation-parameters/

Activation parameter setup.

t-coefficients

Specifies the temperature coefficients in Equation . and Equation ..

u-coefficients

Specifies the U coefficients for Equation ..

y-coefficients

Specifies the Y coefficients for Equation ..

anode-interface

Anode interface options.

cathode-interface

Cathode interface options.

electric-field-model/

Sets electric field.

conductive-regions

Lists zone names and IDs.

contact-resistance-regions

current-tap

voltage-tap

electrochemistry

Sets electrochemistry parameters.

enable-battery-model?

Enables/disables battery model.

model-parameters

Sets model parameters.

by entering define models battery-model. A listing of the various text commands is as follows:

Enters the battery model menu.

Enters the electric field setup menu.

Specifies active conductive regions.

Specifies contact resistance regions.

Sets cathode tap.

Sets anode tap.

Sets battery model options (see Specifying Battery Model Options for definitions of the model general

parameters).

solution-method

Sets solution method options (see Specifying Battery Model Options in the Fluent User's Guide for details).

ntgk-parameters

Sets NTGK model-specific parameters (see Inputs for the NTGK Empirical Model for definitions of the

NTGK model parameters).

ecm-parameters

Sets ECM model-specific parameters (see Inputs for the Equivalent Circuit Model for definitions of the

ECM model parameters).

newman-parameters

Sets Newman model-specific parameters (see Inputs for the Equivalent Circuit Model for definitions

of the Newman model parameters).

parameter-estimation-tool

Computes the model parameters from battery's testing data.You can use the estimation tool to compute

model parameters for the NTGK or ECM model, or for the One-Equation thermal abuse model.You

must provide battery's testing data as a text file in a specific format for each model.When you enable

this tool and select the model option, Fluent will show the required format for the input file in the

console. For more details, see Using Parameter Estimation Tools.You can contact ANSYS Technical

Support for clarifications on how to use this tool.

thermal-abuse-model

Allows you to choose a thermal abuse model and specify its parameters (see Specifying Advanced

Option in the Fluent User's Guide for more details).

Dual-Potential MSMD and Circuit Network Battery Models

Chapter : Fuel Cell Text Commands

This chapter is divided into the following sections:

.. Using the PEMFC Text User Interface

.. Using the Fuel Cell and Electrolysis Text User Interface

.. Using the Solid Oxide Fuel Cell With Unresolved Electrolyte Text User Interface

All of the features for the PEMFC model that are available through the graphical user interface are also

available through text user interface (TUI) commands. The TUI allows text commands to be typed directly

in the ANSYS Fluent console window where additional information can be extracted and processed for

more advanced analysis.

Once the fuel cell module is loaded (see Loading the PEMFC Module), you can access the text user in-

terface through the console window under define/models/pemfc/. A listing of the various text

commands is as follows:

advanced-setup/

Advanced setup.

list-zones-briefly

List zone names and IDs.

contact-resistivity

Set contact resistivity.

coolant-channel

Set coolant channel.

stack-management/

Stack setup.

list-fc-units

List fuel cell units.

create-fc-unit

Create fuel cell unit.

modify-fc-unit

Modify fuel cell unit.

delete-fc-unit

Delete fuel cell unit.

set-stack-current-density

Set the current density on the anode or cathode and modify the current solution to assist conver-

gence. Note: Input here is in units of A/cm2.This is only available if the case contains valid data

(for example, after initialization, iterating, or reading in data). For more information, see IV-Curve

Calculations Using the Text Interface (p. ).

set-stack-voltage

Set the voltage difference in Volts between the anode and the cathode and modify the current

solution to assist convergence.This is only available if the case contains valid data (for example,

after initialization, iterating, or reading in data). For more information, see IV-Curve Calculations

Using the Text Interface (p. ).

reset-setup

Reset the stack setup in case mistakes are made.

submit-setup

Submit the stack setup and makes the stack setup take effect.

anode-setup/

Anode setup.

catalyst-layer

Set catalyst layer.

current-collector

Set current collector.

electrolyte-layer

Set electrolyte layer.

flow-channel

Set flow channel.

micro-porous-layer

Set micro-porous layer.

porous-electrode

Set porous electrode.

cathode-setup/

Cathode setup.

Fuel Cell Text Commands

electrolyte-setup/

Electrolyte setup.

enable-fc-model?

Enable/disable PEMFC model.

Model options.

Model parameters.

reports

Set electrolyte project area and external contacts.

... IV-Curve Calculations Using the Text Interface

For valid case and data files, there are two text commands available to assist in the IV-curve calculation.

These commands are set-stack-voltage (aliased as ssv) and set-stack-current-density

(aliased as ssc), available from the PEMFC text command menu: /define/models/pemfc/ad-

vanced-setup/stack-management/.

Using the PEMFC Text User Interface

For fuel cells, you either prescribe the voltage and obtain the total current delivered by the fuel cell

as a result, or you specify the total current (via flux boundary conditions multiplied by the area) and

obtain the voltage as part of the solution. The details of this IV-relation are specific for each single fuel

cell and depend on mass and heat transport, electrochemistry and inlet conditions, outlet conditions,

operating conditions, and any other parameter or material property involved in the calculation. The

IV-curve is important for applications, because its product is the power delivered by the system.

As described earlier in this manual, you would start a new simulation from fairly static conditions, that

is, high voltage/low current (which implies low species transport and low heat generation). After con-

vergence, you typically may be interested in solutions for new electric boundary conditions, that is,

either for a new cell/stack voltage or current.

In such cases, simply going to the Boundary Conditions task page and changing the value of the

electric potential (uds-) boundary condition, typically allows only small changes, most notably for

stacks. Otherwise the solution will not converge. This is where the set-stack-voltage and set-

stack-current-density commands are important.

In addition to changing the boundary conditions (either to a prescribed voltage or current density),

these commands process the current data in order to estimate the solution for the new boundary

conditions. Because these commands modify the data, you are prompted to save your data, if you

have not already done so.

Before going into details of the commands, here are some general remarks about electric potential

For fixed voltage boundary conditions, both external contacts have a fixed value for the electric potential

(uds-). The anode value will typically be zero, but it does not have to be. The cathode value will be

larger than the anode value and the difference (

) is the positive cell/stack voltage.

For a fixed current boundary condition, one external contact has to have a fixed value and the other

flux boundary conditions. As described earlier in the manual, typically, the anode will have a fixed

(zero) value, and the cathode will be floating, however, you can also set the cathode to a fixed zero

potential, yielding a floating negative anode potential.

The set-stack-voltage command sets the effective stack voltage, that is, the difference (

). For fixed voltage boundary conditions for the previous solution, boundary conditions on both

boundaries are of type fixed value and then the cathode value will be changed accordingly. In the

case of fixed current boundary conditions for the previous solution, the flux boundary condition will

be changed to a fixed value boundary condition, and the value adjusted accordingly with respect to

the other fixed value boundary condition.

The set-stack-current-density command sets the current density on one boundary to the

desired value. Note that the input will be in

, not

as you would normally have to enter in the

Boundary Conditions task page. The reason for this is that average current densities reported in the

text command interface are also in

, and this makes it easier to choose the conditions you would

like to prescribe next. Also, flux boundary conditions entered in the Boundary Conditions dialog box

would have to have a positive sign on the anode side, and a negative sign on the cathode side. The

input for the text interface command is just a positive number, signs are automatically accounted for.

For fixed current boundary conditions for the previous solution, the set-stack-current-density

command changes the respective flux boundary condition accordingly. In the case of fixed voltage

boundary conditions for the previous solution, the cathode side is chosen to be changed from a fixed

value to a flux boundary condition with the new flux.

The two commands may be mixed in an IV-curve calculation. For the type of boundary condition setups

currently described in this manual, boundary condition changes will consistently happen on the cathode

side. However, if anode flux boundary conditions had been chosen initially, switching to fixed voltage

boundary conditions by set-stack-voltage command and then back to fixed current boundary

conditions by the set-stack-current-density command will then have flux boundary conditions

on the cathode side. In this case, using the set-stack-current-density command exclusively

will preserve the anode flux boundary condition setting.

All of the features for the Fuel Cell and Electrolysis Model (sometimes referred to as the Resolved Elec-

trolyte model) that are available through the graphical user interface are also available through text

user interface (TUI) commands. The TUI allows text commands to be typed directly in the ANSYS Fluent

console window where additional information can be extracted and processed for more advanced

analysis.

Once the fuel cell module is loaded (see Loading the Fuel Cell and Electrolysis Module), you can access

the text user interface through the console window under define/models/resolved-MEA-fc/.

A listing of the various text commands is as follows:

resolved-MEA-fuelcells/

Fuel cell model menu.

Using the Fuel Cell and Electrolysis Text User Interface

Set the current density on the anode or cathode and modify the current solution to assist

convergence. Note: Input here is in units of A/cm2.This is only available if the case contains

valid data (for example, after initialization, iterating, or reading in data). For more information,

see IV-Curve Calculations Using the Text Interface (p. ).

suggest-setup

Suggest the stack setup, invoking the automatic stack setup.

Enable/disable fuel cell model.

reports

select-model

Select model.

set-default

Set default.

(aliased as ssc), available from the Fuel Cell and Electrolysis text command menu: /define/mod-

els/resolved-MEA-fc/advanced-setup/stack-management/.

, not

, not

.. Using the Solid Oxide Fuel Cell With Unresolved Electrolyte Text

User Interface

All of the features for the Solid Oxide Fuel Cell With Unresolved Electrolyte Model that are available

through the graphical user interface are also available through text user interface commands.

Once the fuel cell module is loaded (see Loading the Solid Oxide Fuel Cell With Unresolved Electrolyte

Module), you can access the text user interface through the Console Window under sofc-model. A

listing of the various text commands is as follows:

sofc-model/

SOFC model menu

enable-sofc-model?

Enable/disable SOFC model

Set model parameters

Set electrochemistry parameters

Set fuel cell anode interface

Set fuel cell cathode interface

tortuosity-interface

Set fuel cell tortuosity interface

Electric field model

Set voltage tap surface

Set current tap surface

Set conductive regions

Set contact resistance regions

Using the Solid Oxide Fuel Cell With Unresolved Electrolyte Text User Interface

Chapter : Magnetohydrodynamics Text Commands

These are the MHD module text commands available under define/models/:

b0-scale-factor

Set and apply external magnetic field scale factor.

Define MHD boundary conditions

List ANSYS Fluent zone information.

fluid

Set fluid zone boundary condition.

solid

Set solid zone boundary condition.

wall

Set wall boundary condition.

enable-mhd?

Enable/disable MHD model.

external-b0-field

fluid

solid

wall

Set and apply external magnetic field data.

initialize-dpm

Initialize DPM related MHD variables.

initialize-mhd

Initialize MHD model.

mhd-method

Select MHD method.

reset-b0-field

Reset external magnetic field data.

solution-control

Set MHD solution control parameters.

Chapter : continuous-fiber/

All of the features for the continuous fiber module that are available through the graphical user interface

are also available through text user interface (TUI) commands. The TUI allows text commands to be

typed directly in the ANSYS Fluent console window where additional information can be extracted and

processed for more advanced analysis.

Once the fiber module is loaded, you can access the text user interface through the Console Window

by pressing return in the console (assuming that you are at the top level menu, that is, not in any other

menu such as define/). A listing of the various text commands is as follows:

continuous-fiber/

Enter the continuous-fiber menu.

define/

Define fiber models and injections.

injection

Define and modify fiber injections.

model

Select a fiber model.

file/

Read and write fiber data.

read-fiber-data

Read in fiber data file.

write-binary-fiber-data

Write a fiber data file in binary format.

write-fiber-data

Write a fiber data file in standard format.

print

Print the fiber data of all defined injections into history files.

print-xy

Select two fiber variables for plotting into an xy file.

solve/

Solver settings for computing fibers.

compute

Compute the fibers for all of the injections.

print-xy

solve/

compute

Initialize all of the fibers and injections.

set/

Set solution parameters for the fiber model.

Select the discretization scheme for convection terms.

energy

Choose a discretization scheme for the fiber energy equation.

momentum

Choose a discretization scheme for the fiber momentum equation.

species

Choose a discretization scheme for the fiber species equation.

Select the equations that will be solved.

energy

Specify the energy equation that will be solved.

momentum

Specify the momentum equation that will be solved.

species

Specify the species equation that will be solved.

Set parameters for coupled fiber calculations.

Select whether to couple fiber and fluid flow calculations.

no.-of-fluid-iters-per-fiber-iter

Set the number of fluid flow iterations per fiber iteration.

underrelaxation

Set the underrelaxation factor of the fiber source terms in the fluid flow.

monitors/

Set the residual monitors of the fibers.

check?

Choose which currently-selected equations should be checked for convergence.

Set the criteria to stop the fiber calculation.

relative-residuals?

Choose whether relative or absolute convergence criteria will be used.

no-of-iterations

Set the number of fiber iterations that will be computed.

Set the reporting frequency for the fiber model.

Set the underrelaxation parameters.

energy

Specify the underrelaxation factor for the energy equation.

momentum

energy

momentum

Specify the underrelaxation factor for the momentum equation.

species

Specify the underrelaxation factor for the species equation.