Creating symbol w/ redundant pins

Say you have a component that has multiple pins that are internally connected in the part, such as a high power FET with multiple pins for the drain terminal, or a switcher IC with multiple pins for the input…how do you create this symbol?

Ideally only a single pin is created for each function in the symbol…but in the layout I would want the net to connect to all pins associated with this function.

Hi @eeMD this is a good question, and one that comes up frequently.

Currently there is no way in KiCAD to assign a single logical pin on a schematic symbol to multiple physical pins on a footprint. This is functionality that will exist in the future (there is a major rework of the schematic tools underway currently).

Workaround options at the moment:

  1. Add every pin to the symbol - This is the most explicit method, and the suggested approach for the official libs
  2. Change the footprint and give all “similar” pins the same number. Then add a single pin to the symbol and it will be connected to all the same pins on the footprint. This is not the recommended approach as it then means you have a generic footprint that is now application-specific. Footprints should be agnostic to the symbol libs.

As an addendum to 1. there has been some success by placing all symbol pins in the same position on the symbol, and making all-but-one pin “invisible”. This means that only one symbols shows up, but they all are “connected” to the same net as the schematic editor assigns connections based on grid position. However this is certainly not future proof, and is a fairly ugly hack.

TL;DR - You cannot do this (yet).


But be careful if the pin is a power input. then the pin name is used as a label and this pins could be connected to something by accident. (if one uses a label that is the same as one of the pin names.)

Thanks SchrodingersGat. I planned to default to being explicit and adding a symbol pin for every instance but I was hoping there was a clever workaround to avoid symbol clutter.