# RF Ground Stitching in Proteus Ares 8

I am using Proteus Ares 8 to create a PCB for a simple RF circuit. I have a double sided copper board, filled with groundplane on both sides, with a single 50 Ohm microstripline across the board to two SMA sockets, just as an example:

What I am trying to achieve is what is called RF stitching between the bottom and top copper along the edge of the strip-line. Something like the following:

Here I have placed a track alternating between layers, which works, but gets unworkable when the design is more elaborate. I would like to place vias alone, but, then the copper is releaved around the via, because it's not connected to ground.

About the best I can seem to do is to use a small drill hole through the board, set up to be the same size as the via. I can make the hole coated.

However, using this method, I cannot seem to remove the relief around the board. The best I can get is is the thermal relief around the pad, but since my concern is RF grounding, I would like to remove this thermal relief.

In the pad settings, I can select different options for the relief, such as Thermal (shown above) or Thermal-X (45 degree rotated cross), but, I am unable to remove the relief completely with either the Solid or None option.

Any help or suggestions for this would be greatly appreciated.

George, M1GEO.

• Can you set your via's net to GND? Does removing the little linking traces break the via's association with a net? Perhaps copy-pasting one of the vias is a work-around. (I've never used Proteus.) – user2943160 Sep 7 '16 at 1:59
• Sorry for delay. Vias cannot be set to ground directly, because they take on the net from a track - In the first image, see they're connected by a track from the SMA ground. As you ask, removing the track removes the net association. But not with pads. Pads can be set to the GND net directly. Copy-pasting one of the vias is a good idea - I will try and report back. – M1GEO Sep 8 '16 at 11:35
• @user2943160 I tried to copy-paste the via once it was on the ground net, but it takes any traces connected to the via with the copy-paste. See: my attempt here – M1GEO Sep 8 '16 at 12:16
• In the end I used pads modified to be covered with resist and made them the same size as vias, with the plated option selected, and the relief set to solid! The boards have gone off to Fab. The Gerbers looked okay. – M1GEO Sep 9 '16 at 18:33
• Go ahead and write that out as a self-answer to your question, then. – user2943160 Sep 10 '16 at 0:07

Use Pads instead of Vias. Create a component with one pad called Ex: stitchingVia. Place as many as you want in the schematic. and connect them to GND.

in the PCB part View the pad properties and change the Relief to none.

,

Do not connect the pads with tracks. Place a Zone and select the NET to GND and disable the Relief Rins checkbox.

You can create a new pad to use as a via. Someone asked similar questions about Proteus and its uses HERE and LabCenter responded to answer a few questions. The bit you are interested in would be what they say about vias:

"In Proteus, vias are treated as transient objects so they pick up the net to which they are tracked our routed. This connectivity is re-scanned and refreshed when the netlist changes, the project re-opened etc. Stitching to a zone is therefore done with pads. Place a pad, edit and assign to net. Then, either replicate or block copy as required. The clearance will default to that specified in the edit zone dialogue but can be overriden in the pad dialogue itself."

This was also something I was wanting to do before, so am glad I found the response directly from LabCenter. I linked the page in case there were other issues on there you could potentially need some answers to.

For completeness, in Proteus 8.8 and above, Zone Stitching is supported directly by the ARES: See this LabCenter instructional video on YouTube.