1

I know that ground vias along the edge of the PCB can help for the PCB to radiate less (from a EMC perspective). But does it help only for with 4 or more layers PCBs? Or does this also help alot for 2 or 1 layer boards?

And radiate less what? Magnetic fields or electrical fields or radiowaves or what?

How close should the vias be? I guess it depends on the frequency or something?

winny
  • 13,064
  • 6
  • 46
  • 63
martiniko
  • 19
  • 1
  • It's called a via fence. It's supposed to form a Faraday cage in conjunction with ground planes above and below another layer. – DKNguyen Nov 09 '21 at 05:56

1 Answers1

4

The purpose of plane stitch vias along the edge is to counteract the 'slot antenna' formed by planes next to each other. The edge stitch vias seal off this unintentional antenna and blocks EMI that would otherwise escape from the board edge. The vias form a 'picket fence' that looks like a dead short to RF, reflecting it back to the source.

Via spacing for edge stitch should be about 1/8 of the shortest wavelength of interest.

More here: https://www.signalintegrityjournal.com/articles/292-controlling-electromagnetic-emissions-from-pcb-edges-in-backplanes

And here: https://resources.pcb.cadence.com/blog/the-case-for-stitching-vias-on-your-pcb-2

On a 2-layer board you don't tend to have overall planes. Nevertheless it is still be helpful to ensure that large plane areas are bypassed and / or stitched to reduce loop area, especially at the board edge. A top and bottom ground ring around the perimeter is a good idea if your board can accommodate it.

If your design allows it, using the backside as a continuous ground with limits on traces cutting it up (that is, only allow short jumpers when absolutely needed), can work well.

hacktastical
  • 49,832
  • 2
  • 47
  • 138