PCB Edge "via shield" (Faraday Cage) using Altium
To achieve what you want using the via shielding tool:

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 &quot;auto remove loops&quot; in your PCB settings)
Select the track you just laid (select a segment and hit tab to select entire track).
Open the Via Shielding tool and select GND for your net, and check the box for &quot;Selected Objects&quot;; this will limit the shielding to be on either side of your track.
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.
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 &quot;fence&quot;.