1
\$\begingroup\$

I'm designing a board in Altium which uses a micro USB connector however the footprint is giving me some trouble with the DRC.

enter image description here

As seen above the pads are relatively close which causes these tiny strips of solder mask around 0.047mm in width to give errors. I can think of two ways to fix this, either decrease the soldermask expansion to give more clearance OR increase the expansion and remove soldermask along all the pads. Which of these options is "the right way" or does it depend?

Thanks in advance.

\$\endgroup\$

3 Answers 3

1
\$\begingroup\$

Go with removing the solder mask between the pads. It's a common practice for tight spaces.

\$\endgroup\$
1
  • \$\begingroup\$ Ok thanks. I also realised that Kicad which I used to use has zero expansion by default and I have had many Kicad PCBs made and they turned out fine so it should be fine to do it in Altium too. Thanks. \$\endgroup\$ Nov 5, 2023 at 5:26
0
\$\begingroup\$

What is the pin pitch and width? If typical 0.5mm pitch, 0.25mm width, it's acceptable to "shave" pads down slightly to get better fit overall. For example, 0.23mm pad width allows 0.27mm gap, or for example 0.11mm mask web width and 2 x 0.08mm mask expansion.

Whether that's within the exact tolerances of any given fab, or they'll build it with the dimensions as given (risks lower yield), or they override that and build it to their own tolerances -- no idea. Ask your fab if in doubt.

Removing mask between pads isn't a big deal; the chance of solder bridging is lower with mask, but it's still pretty low without, when using proper pad dimensions and pasting. (And pasting doesn't matter a whole lot anyway as the rosin phase melts, allowing it to spread out during reflow; it does still help of course, just to say it's not as specific as you might hope.)

Ultimately, pad dimensions, shape, and positioning are a matter resolved by production. If you aren't doing thousands of units at a time, it doesn't really matter, and sticking to IPC or manufacturer recommended footprints is fine.

The one thing I would recommend at the EDA tool level is setting rounded pad corners, so that the soldermask is also rounded. For typical combinations of trace spacing and soldermask expansion, the trace can overlap the mask expansion region, exposing part of the trace (or if not all the time, then under worst-case alignment). Rounded expansion guarantees it's fine.

\$\endgroup\$
0
\$\begingroup\$

First of all you should check the soldermask capabilities of your PCB fabricator. I never ever remove soldermask between pads, when the fabricator's capabilities support a soldermask web.

Depending on your soldering process and footprint geometry, removing the soldermask entirely ("gang masking") will significantly increase the probability of short-circuits between the pads.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.