If we would speak in general: what is the strength of the solder mask in terms of breaking voltage?

So if we put one PCB with castellated pads on another board like this:

enter image description here

What will heppen if both PCBs would have traces one on another (meaning bottom layer of the top PCB and top layer of base PCB)?

I'd say that it should be OK for low voltage schematics. But what if the voltage is 230 VAC?

  • 1
    \$\begingroup\$ it's not generally OK for low voltage schematics. It depends of what the module does, signal-wise, and what the traces beneath would do. \$\endgroup\$ – Marcus Müller Jun 20 '18 at 8:54

I would advise to prevent traces underneath submodules.
Soldermask is not an excellent insulator, and the thickness may vary.

Aside from insulation, you might encounter interference as well. Especially when these modules provide wireless functionality or power.

When you have to, check the module if there are any exposed pads or via's. And read the datasheet, so you can route around critical area's.

230 VAC, assuming from mains, isn't clean 230V. It already has a higher DC peak, and it will have transients. That would definitely be a no.

But when the module has nothing on the bottom, I have no arguments against it.


Soldermask is basically liquid paint, which means it can have similar defects: varying thickness, and more worrying in your case, pinholes. Its purpose is to prevent solder bridges and protect copper from oxidation, but it isn't specified as a high voltage isolator.

If the module has vias, these will create bare copper areas on its bottom... so all that remains is the soldermask on the mainboard.

Since the module won't be touching the pcb (rather, it will be spaced by the thickness of the soldermask) it would be okay at low voltages... but definitely not 230VAC.

More information here.

Note that if the entire bottom of the module is (for example) a ground plane and the traces you run below it are only a few volts from this ground plane, then it would be OK.

If you must run traces, and this is a one-off or low volume, consider putting some insulating tape on the back of the module, like kapton tape. It should be thin enough not to interfere with soldering the module.

Additionally if high frequencies are involved you'd have to consider noise, due to the capacitance of two parallel plates, and also magnetic (transformer) coupling between tracks on the pcb and on the module.

  • \$\begingroup\$ Just small comment: I can (and I usually do) tent vias with the mask. \$\endgroup\$ – Roman Matveev Jun 20 '18 at 9:52
  • 1
    \$\begingroup\$ hm, I was wondering if that would create thinner soldermask around the edges of vias, and it looks like it does. Check this link and look at the image "Figure 4: A via tented with dry film resist" you'll see what I mean, the mask has trouble around the corners/edges, like any paint would. \$\endgroup\$ – peufeu Jun 20 '18 at 12:21

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.