Default Soldermask Stop

[Sparky49]

Hi,

I've just received a batch of PCBs with soldermask covering many of the pads. Fortunately I was able to scrape this off so this run isn't useless, but it seems I have changed a setting somewhere which results in the top soldermask stop not being applied when I place a pad in the footprint editor. I have tried searching for what this setting might be, but with no luck. Is there an option I should specifically check, or have I borked this right up?

I am using Altium Designer 14.3.

Thanks in advance.

[r0d3z1]

1) check you gerber
2) check your solder mask expansion rules

[ANTALIFE]

Like r0d3z1 said, check the Gerbers you sent to the fab house. To be safe I would load them into a program other than Altium CAMtastic, like DFM Now (https://www.numericalinnovations.com/pages/dfm-now-free-gerber-viewer)

[T3sl4co1l]

PCB Filter Panel, query:
IsPad AND SolderMaskOverride
PCB Inspector Panel: untick Solder Mask Override.
D, R (Design / Rules), find the soldermask expansion rule, set to a typical value like 3 mil (from pad edge, not hole edge!).

As said, never hurts to check your gerber output either.

Tim

[Sparky49]

Thanks guys, fixed it. Was an error in the soldermask expansion rule. 
 
Normally I would view them on GC Prevue or the JLC Gerber viewer, but on this occasion I skipped that to go on holiday.  It's always that one time it isn't checked eh?  Lesson learned.

[UStralian]

Your fabricator should also have caught this, and if not, you should maybe look for a new fab. You can add notes to your fab drawings to specify that soldermask shall not intrude on any surface mount pads (and make sure the pad master is included in your gerbers). The exception is SMD (solder mask defined pads) where the mask opening is smaller than the pad copper, but these can be identified manually if you ever use them.