I designed a PCB with an IC that has a pitch of 0.5. The footprint solder mask looks like this:
However, the gerber came out with one blob that looks like this:
Why did it do that? Can I stop it? Should I stop it?
I don't usually answer my own questions (and really probably shouldn't on EE), but I think I have some additional details that are relevant to answering the question fully. Please provide feedback via comments or votes for the sake of the community.
PCBWay has the following requirements for the solder stop mask:
The TPS612332 Data Sheet recommends a pad width of 0.28mm and solder mask clearance of 0.07mm all around that pad:
If I have a 0.5mm pitch and .28mm of that is occupied by pads with 0.07mm of mask clearance, then I only have 0.08mm for the bridge (which is less than the 0.1mm minimum for PCBWay).
Which is why KiCad didn't put solder mask between the pads for this particular IC.
Can I stop it? Yes. Just like @Seth said in his answer, in PCBNew, I can click Setup->Pads to Mask Clearance and change the "Solder mask clearance" and "Solder mask min width" to allow the solder mask to appear.
Should I? Well, having the solder mask would likely help prevent shorts between pins due to solder issues. On the other hand, it seems like exceeding the minimum requirements set forth by the manufacturer may also expose risk in the manufacturing process.