Either of these pads is valid, Mr. DRC

[baudot]

Many components have redundant connectors.

Examples: Most pushbuttons have 4 connectors, and as long as you wire through any 1 of 2, you’re good. A clip to hold on a watch battery connects is anchored to the board with either of two SMD pads, and you can use either as your positive connector.

Is there a way in KiCad to set up this kind of pad in the footprint editor?
i.e. Either of these two SMD pads for the battery clip is good, as long as the user wires to one, they can ignore the other and the DRC should be satisfied.

[PCB_Wiz]

@baudot

Is there a way in KiCad to set up this kind of pad in the footprint editor?
i.e. Either of these two SMD pads for the battery clip is good, as long as the user wires to one, they can ignore the other and the DRC should be satisfied.

If you are asking does KiCad recognize internal jumpers, the answer is no.

You can of course have 2 pin 1’s and 2 pin 2’s which allows route to either, but that does apply the net name to both.
You could manually remove the net name, to avoid needing to connect to both, and that will pass DRC, but the next net import will re-attach all pin 2’s.

A possible enhancement could be a ‘connect one of’ / ’ connect all of’ type flag, but what about the case where a specific one needs to be connected first ?

An alternate approach would be to allow a connections layer, such that users can place any traces/rats nest on these, and they do not plot, but do pass connectivity.

That would be useful for multi-connector PCBs on one panel designs.

[pedro]

@PCB_Wiz

You can of course have 2 pin 1’s and 2 pin 2’s which allows route to either, but that does apply the net name to both.

And after the board is routed, change back schematic and footprint to pins 1,2,3,4 with 3 and 4 not connected. This way the DRC is happy, though the workaround needs some effort.

[PCB_Wiz]

@PCB_Wiz

You could manually remove the net name, to avoid needing to connect to both, and that will pass DRC, but the next net import will re-attach all pin 2’s.

Expanding on this some more, I just tried both delete of NET name (disconnects pin) and also rename of pin from 2 to 2nc or 2ic, and that seems to stick fine.
I think that renamed pin will now not connect on a new netlist import, so those are 2 simple edits, on one menu, that should be net-update tolerant to do what you are after.

[Rene_Poschl]

A bit hacky for my taste to be honest.

I think the cleanest option is to create a symbol that has all 4 pins and a footprint including all 4 pads with differing pad numbers. That way you can define in the schematic which pin to connect.

I even doubt this is more work in the long term compared to the workarounds posted here. And it has the added benefit of clearly communicating that this is indeed done on purpose.