I’m working with a fairly ancient version, but I’m seeing the option to change the mask expansion under Dimensions -> Pad Mask Clearance. If you set that, and then use the “Do not Tent Vias” on the plot page, then it will generate the specified mask expansion around your vias. It shows these settings on the Plot page too. Strange you can’t set them from there though.
For your case though, it sounds like you’re wanting the mask to cover part of the annular ring, but not over the drilled hole. You could set the mask expansion as a negative value (like Annular Ring -1.5), but that screws with all your SMD pads too. I think you’ll need to go out of KiCAD and fiddle with the gerbers directly, but shouldn’t be too much trouble.
The easiest way I can think of is to do the following with the help of GerbV (not Gerbview, which comes with KiCAD)
- Export the gerbers and NC Drill file
- Open the NC Drill file in Gerbv
- Go to File >Export RS274X (Gerber), save it as something like mask-holes.gbr
- Open mask-holes.gbr in a text editor, and add 1.5 mm to each expansion. If you’ve never fiddled with gerbers before, the line looks like this:
%ADD13C,0.01*%, with the number after the comma indicating the size (Usually in Inches. In this case, 0.01"). - Using GerbV, open up mask-holes.gbr and the drill file. You should see the nice expansion. Close this, or correct anything you need.
- Open up mask-holes.gbr and the top mask layers. Go to File > Export RS274x (Gerber) Merge, and save it as the top mask file.
- Repeat for the bottom.
Done! If you’re on a command-line friendly system, you can replace a couple of these with GerbV’s helpful command line options as well. If you’re having to re-plot a bunch of times, probably not a bad idea to script it.