How do I mark pads on the PCB footprint as not used in KiCad?

Question

I'm using KiCad to design a PCB. I'm using Raspberry Pi Pico, which has a number of GND pins (for designer's convenience).

The symbol/footprint I have (downloaded somewhere from the Internet) have only one GND pin on the schematic, but multiple pads on the footprint.

I have connected two of the GNDs, but the design rule checker complains about other GNDs not connected:

For now I'm just ignoring DRC errors, but this have a downside of making an error and ignoring a legit error hidden between multiple false-negatives.

How can I notify KiCad, that I don't want/need to connect those auxiliary GNDs?

Answer 1

This needs to be done in Schematic Editor prior to switching to the PCB Editor. In Schematic Editor find the No-Connection Flag icon, (short line with an "X", in the right sidebar), click it, then drag a No-Connect X to the schematic pin that will be a No-Connect. Later when that component transfers to the PCB Editor there will be no net name on that pin, so no trace is needed.

(In KiCad 6 you can also place the cursor on the pin and press a "Q".)

Answer 2

The footprint must correspond to the symbol. If footprint has many GND pins then the symbol should have them too.

The usual way of doing this is to mark all but one pin with same signal as invisible, then stack them on top of each other in the symbol editor. Then, when you connect the wire to the visible pin, all the invisible ones will be automatically connected too. This way you will have only one GND in the schematics, but multiple pads on the PCB.

Since you mentioned that there is only one pin on a symbol but DRC complains about extra pads, I suspect this is exactly what has been done in the symbol you've downloaded.

Alternatively you can make all additional GND pins visible and connect them on the schematics (or mark them as NC). I would not recommend doing this with power pins though. It is better to connect all of them.