Author Topic: Does soldermask matter for via-fencing?  (Read 211 times)

0 Members and 1 Guest are viewing this topic.

Online LoveLaika

  • Regular Contributor
  • *
  • Posts: 200
  • Country: us
Does soldermask matter for via-fencing?
« on: May 05, 2021, 06:30:26 pm »
I have some questions about a via fence and soldermask. I was told that a via fence would help against EM interference, so I have ground vias surrounding my circuit. However, if the vias were covered with soldermask, would it render the via fence ineffective? I see why at times soldermask isn't applied to RF PCBs as an example, but I'm not working with high frequencies. Would it be fine if the via fence was covered with soldermask, or is it better to just remove the soldermask even if I'm not working with high frequency signals?

Offline ejeffrey

  • Super Contributor
  • ***
  • Posts: 2452
  • Country: us
Re: Does soldermask matter for via-fencing?
« Reply #1 on: May 05, 2021, 07:37:05 pm »
No it's fine.

The purpose of the via fence is to short out waveguide modes propagating through the interior of the board.  External surface treatment has no effect.  Also, the whole point is to have no signals in the area of the via fence, so it isn't sensitive to loss or impedance.

Solder mask is often cut away near exposed transmission lines such as microstrip or CPW because they have substantial fraction of their energy in fields above the board.  Solder mask adds an uncontrolled dielectric which can change the impedance and add unwanted loss.

Offline radiolistener

  • Super Contributor
  • ***
  • Posts: 1745
  • Country: ua
Re: Does soldermask matter for via-fencing?
« Reply #2 on: May 06, 2021, 05:10:17 pm »
Would it be fine if the via fence was covered with soldermask, or is it better to just remove the soldermask even if I'm not working with high frequency signals?

For RF frequencies it depends on where vias are placed. Soldermask is critical over RF transmission lines. If your vias are not a part of transmission line (for example - vias around transmission line), then soldermask doesn't matter.

For RF transmission line soldersolder mask is critical, because it's properties very depends on the factory and even on the PCB instance. So it's better to not cover transmission line with soldermask to avoid unpredictable parameter dependency from PCB instance. If you still needs soldermask over transmission line, as I know there is a special soldermask material exists, which RF properties are more stable. But I think it will be hard to order PCB with such soldermask material.

If your circuit don't works with RF frequencies it doesn't matter. Even for a short wave frequencies (below 30 MHz) you can put soldermask over transmission line and it's effect will not be noticeable.
« Last Edit: May 06, 2021, 05:36:20 pm by radiolistener »

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 17137
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Does soldermask matter for via-fencing?
« Reply #3 on: May 06, 2021, 08:35:54 pm »
I mean, it's not really... "critical", you can put soldermask over a 30GHz microstrip just fine... maybe the attenuation is a couple tenths of a dB/mm worse or something, unlikely a deal breaker in a lot of applications.

Resonant structures -- filters and matching -- are more susceptible: simply, they have more reactive power (or high SWR), so more power can be lost through the electric field losses in the soldermask.  These are more likely places to have some effect.

Or maybe an application is high precision, so those fractional dB can't afford to be lost, even at SWR --> 1.  Maybe that's where you're coming from.  Dunno, you didn't say.  And you didn't give any numbers as far as attenuation with/out.  So it's all just a bunch of hearsay.

Personally, I would give a very different motivation: I prefer tented ground stitching vias, because they look cleaner, and don't have a risk of shorting to nearby pads during wave soldering.  Fields by the vias are almost irrelevant, as mentioned above.

Put another way:

If you're doing something high enough in frequency that you need a PCB EM field solver to design it, you might as well tick on the soldermask material properties and include that in the simulation.  Then you can solve two things at once: 1. what, if any, error (in terms of tuning shift due to the slight increase in capacitance) the soldermask contributes, and 2. whether it should be removed or not (due to excessive losses).

With that, no one else has to tell you what to do, you are fully in control of your design, and you have complete testable results at your fingertips.  The only thing that may be missing, is the time needed to set up that test plan.  YMMV.

If you're not using a field solver, you're probably doing something very much more basic, like hooking up an antenna to a 50 ohm transceiver module.  For which, the manufacturer will provide guidelines how to do that.  Again, no need for anyone else to tell you what to do.

And if you're not doing either of those, yeah, likely it doesn't matter one lick!

Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!

Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo