7
\$\begingroup\$

Here is a photo of one of Texas Instrument's RF EVMs.

enter image description here

Please pay attention to edge of the PCB that has multiple tiny holes. I marked 3 of them with a red circle on the photo.

What is the purpose/benefit of them? The edges are V cut, is it something to do with it? Or if it is kind of performance improvement, then how do you determine what size of the hole to use and the distance between the holes?

EDIT:

Here is the gerber view of the board (not the same edge), as I can see, they are just holes (not vias)

enter image description here

\$\endgroup\$
  • \$\begingroup\$ Related electronics.stackexchange.com/questions/116518/… \$\endgroup\$ – Matt Young Nov 28 '14 at 22:12
  • 1
    \$\begingroup\$ "as I can see, they are just holes (not vias)" A via is a hole - it just happens to be plated. How can you tell from that if they're unplated? They look just like all the other vias to me, especially all the ones under the chip. \$\endgroup\$ – Majenko Nov 28 '14 at 22:27
  • \$\begingroup\$ under chip holes are plated, the other ones should be plated as well. \$\endgroup\$ – Angs Nov 29 '14 at 10:20
12
\$\begingroup\$

Those are vias. They are connecting that one piece of ground plane to another one on another layer.

It may be done for increasing current carrying ability, thermal transfer, EMI reduction, and any number of other reasons.

Given that it's an RF board it's most likely to help control unwanted EMI.

When you have two ground planes, and high frequency, different points of the ground planes will be at different voltages, with respect to each other. 0V is never 0V throughout an entire system, but varies due to the inductance of the traces.

Two traces with different high frequency signals in them make a nice dipole antenna. By strapping those two traces (ground planes) together you are effectively nullifying much of those voltage differences, and turning it back from an antenna to just a ground plane. And of course the effect is most pronounced at the edges of the planes, so that's where you want most of your vias. You notice there are also plenty of vias throughout the whole ground plane in an attempt to keep the potentials as even as possible.

\$\endgroup\$
  • 1
    \$\begingroup\$ Any reason why they would be along the edge in such quantities? \$\endgroup\$ – geometrikal Nov 28 '14 at 21:36
  • 8
    \$\begingroup\$ Being so close to the edge and so close together makes it seem as though they're for reducing EMI leaking out the edge from inner layers, sort of like a grounding cage. \$\endgroup\$ – Ignacio Vazquez-Abrams Nov 28 '14 at 21:36
  • 2
    \$\begingroup\$ This is most likely for EMI shielding. Along with ground planes and copper pours, these vias form a shield around sensistive signals. \$\endgroup\$ – Nick Alexeev Nov 28 '14 at 22:23
  • 1
    \$\begingroup\$ Could anyone please explain the theory behind it how the vias on the edges improves the EMI performance? Is it a common method on RF devices? Does this method have a name? How do you determine how many holes to use on the edges and the distance between them? Would it improve the performance more if TI doubled the number of the holes on the edges (although it would slow down the production)? \$\endgroup\$ – Angs Nov 29 '14 at 10:18
  • 2
    \$\begingroup\$ @angs: The holes in a Faraday cage determine the wavelengths of EMI that are absorbed; making them smaller than the smallest waves doesn't make it much more effective. \$\endgroup\$ – Ignacio Vazquez-Abrams Nov 29 '14 at 15:27
11
\$\begingroup\$

It's called via stitching, a via fence or a picket fence.

It's typically used to control EMI at very high RF frequencies- getting in or getting out, and can also reduce the resistance of the connections at DC.

If the copper areas are joined by more widely spaced vias the loop area and inductance would be higher, and at DC more vias in parallel mean a lower resistance.

Edit: Here (from Wikipedia commons) is a photo of an RF board (an LNB).

http://upload.wikimedia.org/wikipedia/commons/3/33/LNB_dissassembled.JPG

\$\endgroup\$
  • \$\begingroup\$ do you have attribution for the picture? \$\endgroup\$ – placeholder Nov 29 '14 at 17:42
  • \$\begingroup\$ @placeholder It's linked through the Wikipedia page I had already linked to, but I'll add it in the image description. \$\endgroup\$ – Spehro Pefhany Nov 29 '14 at 17:49
5
\$\begingroup\$

Three are three reasons why the "picket fence" or "Via stitching" is done at the edges.

1) The dominant reason is to reduce EMI, Consider it a small Faraday cage for your board. This has been covered in other answers so there is no need to elaborate further.

2) For ESD reasons. Good board design dictates that you have a ground ring around the periphery of your board. Boards are handled by their edges and in having a ring around the edge any potential ESD events get dumped into a solid ground, get conducted around the circuits and onto where ever it wants to go. Once in use this rail/ring also helps move any ESD events into connectors to the edge of the board and away. Having ground on both sides and at the edge is a more complete version of a ring and also reduces the resistance.

3) Mechanical reasons. These vias stiffen up the board. Notice that I didn't say make it stronger. When you flex a board, often the shear planes between layers tear apart vias and cause disconnects. Adding vias could very well weaken the board (in it's ultimate yield strength, you have to assess each design individually). But what it does do is make the board less flexible. i.e.; stiffer. That prevents the whole board from flexing during handling and particularly poor handling (picking a board up one handed by one edge) and moves the stress out to the edge where there is no critical vias (or at least redundant ones) and prevents flexing in the inner areas where there might only be one via.

\$\endgroup\$
1
\$\begingroup\$

As already stated in the comments it is shielding. See http://webbooks.net/freestuff/EMCDesignGuideforPCB.pdf, page 53.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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