Can't Connect Pads on Same Net

[braddrew0]

Hi Guys,


Struggling with KiCad (pcbnew). I can't connect two pads on the same net. I understand that it's likely a design rules violation but I'm unsure which rule is the problem (nor whether I can change it). The first picture shows what happens when I try to connect from an outside pad to the offending one, the second shows when I try to connect in reverse. The footprint is for a CUI RCA connector (footprint sourced from EasyEDA via Digikey) and I have a ground plane on the bottom - so the pad should already be connected. I have other through hole components which have successfully connected to the ground plane - this is the only one I'm having any trouble with.

Any ideas which setting is the likely offender?

Thanks!


Brad

[EEEnthusiast]

Check the oblong pad if it has copper on both sides.
Check if there is any keep-out zone surrounding the pad

[poeschlr]

You could try and run "cleanup tracks and vias" tool as there might be a short track hidden somewhere. (could be caused by https://bugs.launchpad.net/kicad/+bug/1840177)

If that does not fix the problem inspect the footprint. Maybe there is more than one pad at the place you try to connect.

Another option is that the footprint somehow has something on the edge cuts layer (some footprint suppliers define oval holes that way. This would not be compatible with version 5 of kicad as edge cuts are taken into account for DRC)

[braddrew0]

Thanks guys - there were hidden edge cuts underneath the pads! Appreciate the help

[bson]

Another possibility in general when running into something like this is a combination of settings:
1. Snap to pad is disabled in preferences
2. The grid is set too coarse for a gridpoint to coincide with the pad

This can happen if you have the snap setting disabled and used the grid for positioning previously.