Arduino common GND


I started with Arduino a few weeks ago and while making the PCB board I noticed that in the schematic symbol of the UNO I used the GND connections (3 of them) even being common ot the same in the UNO in the schematic symbol they appear to be 3 different connectors.

How can one define common grounds or common pins in a schematic symbol ? in order to hace common connections without need in the PCB to route them individually.

Thanks and regards Rainer

You are referring to the Uno shield symbol which has 3 ground pins.

There are 3 ground pins, because the Uno shield has 3 ground pins. Best practice is to connect all of them in the schematic and on the PCB.


In kicad there is no way to define that a pin of the symbol connects to multiple pads (with different pad numbers) of the footprint.

One can either show all pins in the symbol as done by the symbol shown in the screenshot, or one can stack the pins. (Stacking means one pin is visible all others are invisible. All pins moved on top of each other.)

For power pins one needs to be careful when stacking. Do not give the hidden pins in the stack the electrical type power input. A hidden power input pin behaves like a global label. The solution is to give only the visible pin the type power input and the hidden pins the type passive.

There is a problem though. The library editor does not like this. One needs to setup the pins correctly before stacking them. (Opening pin properties of any stacked pin changes all pins in the stack to have the same electrical type and pin name.)

Stacking output and power output needs to be done in a similar manner. In this case not because hidden pins are labels but because connecting multiple output pins results in ERC errors.


Hi and thanks everybody.

regards Rainer