Insufficient Soldermask Clearance


I’ve uploaded my Gerber files to for a check (as was suggested here) and I got a zillion remarks back about “insufficient soldermask clearance”.

At first, it was not clear to me what this meant, but then I came to know that it’s caused by the fact that the solder mask is equal in size compared to the footprints of the components. I found out that the “solder mask clearance” is by default set to 0 in KiCAD (Dimensions -> Pads Mask Clearance). Hence, the equal size of footprints and solder mask.

What’s the general rule here? Should/must the solder mask clearance be bigger than 0 and if so, how much? If you forget it/don’t do it, what could be the consequences? After all, there must be a reason why gives me so many warnings and they advice me to set the solder mask clearance to 0.003"…

You’re probably OK with ignoring those errors, but setting it to 3 mil is a good idea.

The issue that it’s warning you of is mask registration errors. When the fab puts the mask on there, it can potentially be slightly off, so the whole mask layer is shifted relative to the pads. This picture is a good example of this. The 3 mil mask clearance ensures that if there’s a shift, then it doesn’t cover up the pads (or at least minimizes the damage). It’s also possible for the mask features (eg, the hole over the pad) to be shrunk or enlarged slightly, but typically this is covered by the same spec.

However, this is NOT a case where bigger is always better, since excessive mask clearance can pose issues as well. As an example: If you have a board with 6 mil trace spacing, a 5 mil mask clearance, and a 3 mil mask shift, you get something like this:
As it looks in the design tool
Worst-case scenario from the fab
In this case, the fab is within spec, but still manages to expose the ground plane right next to your pad. Still usable, but it’s a bad situation that will lead to shorts if you’re not incredibly careful. This is mostly an issue if you’re not careful about mask as you decrease isolation, but it’s a really nasty trap.


Great explanation and nice examples. Thanks a ton!