I am trying to add a "via shield" to my PCB edges, which is also called a Faraday cage.

enter image description here

I am trying to add vias using Altium software, but the vias are added outside the PCB edge and not inside.

Any idea how to add vias inside the PCB edge?

enter image description here

enter image description here

Above are the settings that I used for via stitching. Can anyone tell me what settings I need to use, to add the shielding vias inside the PCB edge?

  • 3
    \$\begingroup\$ Try the add stitching vias feature instead of "add shielding". Alternatively, just set a convenient grid and manually place vias on the grid points. \$\endgroup\$
    – The Photon
    Feb 11, 2021 at 22:23
  • \$\begingroup\$ May I ask when this is actually required? What kind of designs need such caging and how effective it is? Never saw PCBs with vias along the edges. Would appreciate if anyone sent some link to clear and understandable explanation and usecases (basics would be enough) \$\endgroup\$
    – Ilya
    Feb 11, 2021 at 22:31
  • 2
    \$\begingroup\$ @Ilya It's required in RF designs as the gap between layers can function like a waveguide at high frequencies and the VIA fence creates inductance to block RF from leaking out from between planes. It also keeps everything at the same potential. \$\endgroup\$
    – Voltage Spike
    Feb 11, 2021 at 23:15
  • 1
    \$\begingroup\$ @llya Rick Hartley talks about this in one of his lectures: youtu.be/ZYUYOXmo9UU?t=5220 \$\endgroup\$ Feb 12, 2021 at 0:30

2 Answers 2


To achieve what you want using the via shielding tool:

  1. Lay a track around the outer perimeter of your pcb but offset from the edge, assign it to the GND net. (You may need to uncheck "auto remove loops" in your PCB settings)
  2. Select the track you just laid (select a segment and hit tab to select entire track).
  3. Open the Via Shielding tool and select GND for your net, and check the box for "Selected Objects"; this will limit the shielding to be on either side of your track.
  4. Configure the via sizing and spacing as desired and click ok to apply. You should have vias now on both sides of your track, with net GND.
  5. Select and delete the track. The vias will remain in place. You can delete the inner row of vias if you desire only a single "fence".

I tried @gcr method. It works very good! Here is how I did with screenshots:

1 - Copy/paste board outline track on top layer

2 - Shelve all polygons (t + g + h)

3 - Assign the copied tracks on GND signal enter image description here

4 - Add shielding vias to GND enter image description here enter image description here 5 - CTRL+H to select the GND track around you PCB and delete it

6 - Restore all polygons (t + g + e) and repour all (t + g + a) enter image description here

Here is the result: enter image description here


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.