3
\$\begingroup\$

I am designing two boards that are supposed to operate at frequencies 2.45GHz and 5.8GHz.

In my design, I use simple microstrip lines (not coplanar) on FR4 substrate.

There are some quarter-wave transformers in my circuit and I was wondering how to optimize the surface finish.

I decided to remove the silkscreen from the top layer to cover it entirely in ENIG gold finish as the area of traces is quite small. However, the bottom ground plane is almost solid and covering it in ENIG is going to increase my prototype production costs.

Should I cover it with a solder mask (there will be probably some additional losses) or bear the costs? The manufacturer does not allow raw copper finish, only soldermask, ENIG or lead/tin.

Board: enter image description here

enter image description here

\$\endgroup\$
1
  • \$\begingroup\$ I've never heard of a board done with different finish on the two sides. Are you sure your board shop even allows that? I've also never heard of the cost of ENIG depending on the exposed copper area, certainly not in prototype quantities. \$\endgroup\$
    – The Photon
    Sep 27 at 14:46
5
\$\begingroup\$

The important side of the ground plane is the one facing up toward the microstrip lines.

Coating the bottom with solder mask will have no effect at all on your RF performance. So the simple solution is just to do that.

\$\endgroup\$
2
  • \$\begingroup\$ Thank You for the explanation. What about antennas? If I would like to produce a patch antenna the ground plane can also be left without a solder mask too or the situation will be different? \$\endgroup\$ Sep 27 at 15:25
  • 1
    \$\begingroup\$ @Marcin_Wachowiak, Yes, if the fields are mainly between the ground plane and the patch feature, and radiating "upwards", then a solder mask layer on the bottom side of the ground plane is going to have no effect on the antenna performance. In an F antenna (where you remove ground from under the antenna) the solder mask on the bottom side would cause a disturbance in the radiation pattern. \$\endgroup\$
    – The Photon
    Sep 27 at 15:29
3
\$\begingroup\$

Good for you for thinking about every detail!

With ENIG, the gold finish will be so thin that the nickel content dominates. Nickel is ferrous and quite lossy and thicker than skin depth I suspect. Just don't sweat the finishes.

There are low roughness foils you can order to smooth the underside, which can help losses but it's typically adds a good bit of cost and has a modest impact at 5GHz.

Unless you are REALLY focused on slight losses or reflections, just define the impedance of the lines and let the board house manage hitting impedances by ordering with impedance tolerance.

There are too many variables that you can't predict - metal thickness, etch profile, resin content, dielectric thickness, glass weave, etc

For loss, unless you have reason to be chasing a dB, the standard manufacturing flow will be fine.

\$\endgroup\$
0

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.