Why solder mask are not applied to RF PCBs

Question

I've gone through some of the RF PCB designs. In which solder masking on the traces are not present. Like this one

Is there a specific reason or performance issue to remove that?

Soldermask is lossier than air. – The Photon Jun 23 '18 at 06:12 — The Photon, Jun 23 '18 at 06:12
We have used 1.5GHz signal but with soldermask itself. – User323693 Jun 23 '18 at 07:14 — User323693, Jun 23 '18 at 07:14
ahhhh RF PCB design is really pretty – user371366 Jun 24 '18 at 01:10 — user371366, Jun 24 '18 at 01:10

score 28 · Accepted Answer · answered Jun 23 '18 at 06:30

28

There are several reasons.

1) Soldermask is lossy, and different types of mask are differently lossy. So having no soldermask where the RF fields are gives the best transmission, and if your board is made by different fabs, the most repeatable transmission.

2) Line dimensions, which affect characteristic impedance, are critical. It's difficult to optically inspect them if they're covered with resist.

3) In development, you might just want to add an attenuator pad, or pickoff resistor, to the line. This is tricky enough as it is, without having to start by scraping resist off.

answered Jun 23 '18 at 06:30

Neil_UK

158,152
3
173
387

1

I have a hobby interest in electronics, but nothing professional. Could you explain what you mean by "lossy"? What's being lost? – Alexander Jun 25 '18 at 01:28
4

Microwave power. Dielectrics can be characterised by how badly they absorb energy as a result of an alternating electric field across them. Materials like FR4, the standard PCB substrate, are usable to a few GHz. Solder resist is not designed to be a 'good' dielectric, just reasonable, but to resist solder, and be easy to apply. Where a designer is pushing the limits on line attenuation with frequency, he'll leave out the resist. Sphero's reply about its effect on capacitance is just as relevant, with the poorly controlled thickness changing the characteristic impedance of the track. – Neil_UK Jun 25 '18 at 05:11

score 20 · Answer 2 · answered Jun 23 '18 at 08:35

In addition to the reasons given by Niel_UK, there is the matter of predictability and modeling.

Soldermask is applied as a liquid. As such, its thickness may not be as well controlled and predicable as the thickness of the substrate and conductor layers. In addition, it may have an unpredictable profile - how does it "flow" in between the traces? All of this means that you cannot accurately model the impact of the solder mask on your line, and cannot predict the impedance of the trace.

This is even important on any distributed element filter or microwave component such as a directional coupler, resonator, power combiner, etc. In these cases, a very small shift in the \$\epsilon_{eff}\$ of the system will potentially shift the center frequency out of the band of interest.

With high-performance RF substrates we can get very accurate models, provided we know very precisely the etch profile of the process. The unpredictable nature of solder mask ruins this.

score 12 · Answer 3 · answered Jun 23 '18 at 14:47

12

Aside from the lossy nature, solder mask has a high dielectric constant relative to air and poorly controlled thickness, so the characteristic impedance will be harder to control with solder mask applied. Zo decreases by about 1 Ohm / mil of soldermask thickness. LPI solder mask affects Zo by about 2 ohms and dry film by as much as 7 ohms.

answered Jun 23 '18 at 14:47

Spehro Pefhany

376,485
21
320
842

4

Cool, so one could tune transmission lines with soldermask spray? :) – rackandboneman Jun 23 '18 at 14:52
2

@rackandboneman In one direction (down) anyway... unless you have some material with \$\epsilon_R\$ < 1. – Spehro Pefhany Jun 23 '18 at 15:03
3

@rackandboneman Yeah! But I find it easier to use finger grease applied accurately while holding my tongue at the right angle. :-D – LorenzoDonati4Ukraine-OnStrike Jun 23 '18 at 15:20

Why solder mask are not applied to RF PCBs

3 Answers3