I’d like to make pads with two drill holes. The footprint editor’s Pad Properties doesn’t have options for more than one hole. Is this possible at all?
Any pointers or ‘workarounds’ welcome!
PS: footprints with overlapping pads create the desired layout, but ERC complains about pads on the PCB that don’t fit the schematic. Currently my best solution is to create parts with two connected pins corresponding to two non-overlapping pads (joined with a trace in pcbnew). But that looks ugly in the schematic…
Usually fab houses create PTHs for drill holes that are sitting in copper, even NPTHs.
So the easy way out would be to place a NPTH on the copper pad area of a PTH in the footprint editor like that: z_Solderpad_2.4x1.4.kicad_mod (484 Bytes) (be aware that I haven’t tested this functionality yet, as it’s on my current board that didn’t see a fab yet)
The other way is to make slightly overlapping PTHs in the footprint and give them the same pin number/ID to get DRC on board like this: z_Solderpad_Large.kicad_mod (1.5 KB) (this one works, tested on a board that came back as desired and DRC doesn’t complain)
pad number 3 is actually TWO pads - BOTH of them are identified as Pad Number “3”. One pad is identical to pad number 1; the other is identical to pad number 2. Set the X and Y locations to create pad number 3 with two holes, as shown.
The KiCAD DRC treats overlapping pads as a single pad if there is enough overlap. I have used rectangular SMT pads to create the necessary overlap when there is a significant separation between pads. I don’t know if there is a limit to the number of pads that can overlap.
You can also study the composition of “Pad 2” - which has both a PTH and a NPTH - in the atch footprint for a TO-220 package.
And when you create the pads like that (overlapping, etc.) it’s a good help to switch the pad fill mode off on the left hand side toolbar, as otherwise you can’t really see what you’re doing.
Looks then something like this and makes it easier:
