3

How do you choose the size and the parameters related to via stitching and shielding when you need to create a shielding on pcb around a RF micro strip?

OPTION A

enter image description here

OPTION B

enter image description here

chris
  • 1,553
  • 5
  • 23
  • 42

1 Answers1

3

The via diameter is not critical to the shielding performance (for designs I've worked on). Just having a conductive path between the ground planes on different layers, spaced not too far apart, is what provides the shielding.

So the choice is based on other concerns. Small diameters cost slightly more (below about 12 mil, anyway), while larger diameters take up more space that you might want to use for routing or parts placement.

If you're going to mount a metal shield onto your PCB, of course you need to provide some vias/through-hole pads of the correct size to mount the shield.

Edit RE: "option A" and "option B":

  1. Thermal relief is only needed when you're going to solder something into the hole. I have no idea why Altium gives thermal relief as a default, especially since they clearly distinguish between pads, which sometimes might need thermal relief, and vias, which practically never should. So, definitely option A, but also get rid of the thermal relief on the other vias where it isn't needed.

  2. You should not be using blind vias if you don't have a good reason to pay for them.

  3. Your tracks are likely short enough that you don't need to worry too much about maintaining controlled impedance. Unless you are working above maybe 2 GHz.

  4. If you are working above 2 GHz, then the fact your SMT pads are much larger than the trace is a bigger issue than the spacing or size of the fence vias. You'd want to adjust your layer thickness to give a trace width as close as possible to the dimensions of the pads that are connected to that trace, to avoid the pads having excess capacitance.

The Photon
  • 126,425
  • 3
  • 159
  • 304
  • Does the via need to go from top layer to bottom layer, or do they need to go from top layer to ground plane layer ? – chris Jun 23 '16 at 04:24
  • It needs to surround whatever you're trying to shield. But it's much cheaper to just make them go all the way through the board. – The Photon Jun 23 '16 at 04:31
  • So they don't need to be connected to the ground plane ? – chris Jun 23 '16 at 04:46
  • Yes, they need to be connected to the ground plane. That's what provides "surrounding" the sensitive parts from below. – The Photon Jun 23 '16 at 04:49
  • Thank you. This is the information I needed confirmation. They go trough all but are still connectd to ground plane – chris Jun 23 '16 at 04:52
  • how you establish the distance neeed between each via ? – chris Jun 23 '16 at 04:53
  • Should be well less than 1/4 wavelength of the signal of interest. 1/10 wavelength is great if you can do it. – The Photon Jun 23 '16 at 04:55
  • One more question: when you use the shielding function of Altium it will ask to select a net to place the shield around, however in some case (and in mine particularly) there are some component between the connector of my module and the connector of my antenna. In a result there are no net present on the connector and Altium doesn't place any via for shielding at proximity of component (as not designated as net). Is it critical and how do you handle this problem ? – chris Jun 24 '16 at 03:48
  • @chris, I rarely use Altium's auto-placement features. I'd manually place the shield vias. – The Photon Jun 24 '16 at 03:51
  • After you have placed the shielding via, we need to pour the polygon where the via are inserted, correct ? If yes, then it create some hole around the via, is it normal ? – chris Jun 24 '16 at 04:20
  • You need to assign the same net to the vias and to the polygon. If you place the polygon first, the vias might get automatically assigned the same net (or maybe not, the ways of Altium are sometimes mysterious). – The Photon Jun 24 '16 at 04:31
  • My question is after the via are placed, Altium ask me if I want to repour the polygon. If I click Yes, then the via are connected to the top plane via a cross pattern with 4 connection creating also some "empty of plane" areas between those 4 legs. I am concerned about those empty areas who are created as around my strip it makes that S distance between the strip and the edge of the plane is not respected anymore. Should I repour the polygon with those empty areas or should I not repour ? I have added picture to the question with both option, may be you will better understand my question. – chris Jun 24 '16 at 05:02
  • Those cross patterns are called *thermal relief*. You can get them to go away by changing a design rule, though I can't point you to the exact one (search for "Altium polygon connect style" for more details). – The Photon Jun 24 '16 at 05:06
  • I found the rule to do so, this is in plane part. I just want to know if I should keep those thermal relief or not ? – chris Jun 24 '16 at 05:21
  • @chris you do not need thermal relief on vias. – efox29 Jun 24 '16 at 06:52
  • For effective shielding, you *do not want* any thermal relief on the vias. Solid adjacent ground copper is part of the goal. – user2943160 Jun 25 '16 at 02:20