Zone vs. Soldermask clearance collisions at corners (lp:#1563744)
Original report created by Paul "LeoNerd" Evans (leonerd)
If you place an SMT pad in a zone, due to the way the zone clearance gets
rounded corners it can mean there's a little bit of copper that overlaps
into the pad area.
For example: the attached screenshot shows a zone of clearance 0.01in
inside which is placed an SMT pad of mask clearance just under 0.008in (the
actual value 0.007874015748in being 0.2mm). You would expect that this is
perfectly safe; a nice 0.002in of safety margin between the solder mask
opening and the copper zone.
But you'd be wrong. The problem is that the zone clearance only applies
vertically and horizontally from the pad; the cleared area within the zone
gets a rounded corner of radius 0.010in, meaning it could only guarantee
clearance of a square corner at most 0.00707...in (0.01in * sqrt(2)) wide.
The mask clearance of 0.008in gives a tiny margin of bare copper from the
filled zone exposed within the pad clearance area.
This isn't just a rendering issue; I have had a bad copper run of boards
from the fab because of actual spilled out copper in these pad areas,
causing grounding shorts to the pads when soldered.
As a workaround for these collisions I've been manually editing the per-pad
Cu clearance settings and increasing it on any pad that would be affected.
I'd prefer to leave the global zone clearance at a nice small 0.01in though
because I need to route some grounding pour between TTH connector pads, so
that can't be too big.
Original tags: pcbnew