The included image shows my problem. I’ve tried messing with all of the Zone settings and double checked the footprint/pads don’t have hidden individual clearance settings (they’re all the same). I have tried adding a trace connecting GND pads on the In1 layer to give the zone something to work off of (even though it should work with all the through-holes anyway) but no change.
Did you try to refill using the shortcut B or by running DRC?
Yes, tried refilling many times using “B” each time between adjusting settings.
At this point I’ve got to assume you’ve shut down Kicad and reopened it? This isn’t making much sense at this point. Is this a design you can share for others to look at or maybe post more of it?
What version and OS are you using? Under the help menu there should be an option to copy the version info to the clipboard.
Edit: Just grasping at straws with this one but sometimes switching canvases cures things. F9 and F11 should do.
Is this your own footprint? There may be some pad errors
Found the issue.
The Edit Pad dialog shows “All copper layers” for all pads, as it should. However, in the kidad_mod file, I see a small difference. Take, for example, pads A3 (working properly):
(pad A3 thru_hole circle (at -9.64946 -1.24968) (size 1.27 1.27) (drill 0.6985) (layers .Cu F.Paste F.SilkS F.Mask)
and pad B3 (not working):
(pad B3 thru_hole circle (at -9.64946 1.24714) (size 1.27 1.27) (drill 0.6985) (layers F&B.Cu F.Paste F.SilkS F.Mask)
Changing “F&B” to "" on pad B3 fixes the issue for that pad. I either didn’t design this footprint and found it online or designed it several years ago and don’t remember doing it. I found the footprint in an older project of mine and imported it into this new project.
I guess this may have originally been a KiCAD legacy footprint file and the conversion to the pretty format didn’t consider it would be used for more than 2 layers and only put “F&B” on some pads?
Thanks for everyone’s input which prompted me to look at the contents of the kicad_mod file and ultimately find the problem!
KiCad is a bit limited in handling footprints that have different pad shapes on different layers.
This may not have anything to do with your current problem but not sure why the paste layer is enabled. This is a through hole pad.
1 Like
Ahh yes, thanks. I did notice the paste layer was on and I don’t remember doing it so maybe another artifact from the conversion? I caught it while fixing the initial problem and did a find/replace to remove it from all pads in the kicad_mod file. Thanks for your review though!
Did you notice the front mask is enabled but not the back mask? And there’s a front silkscreen layer enabled for some reason. Had to fix those too 
. Everything looks good now after checking each layer in gerbv.
1 Like
What’s odd about having a front silkscreen? Most parts need that one.
I think he means that some pads had F.SilkS enabled.
Right, the pads had it enabled which showed up as a circle around each front pad. For a PCIe connector those wouldn’t aid with assembly and they’d be underneath the connector once assembled.