KiCad 7 Alternate Schematic Symbols: How to Create Them

This FAQ is about regular and alternate schematic symbols in KiCAD, a feature that can be extremely useful.
It is only possible when using Personal Libraries, the reasons are explained in this FAQ:

Read it first.

Is there an alternate symbol functionality in KiCAD?

Yes, it’s there, but it has a non-obvious name: De Morgan.
Originally made for logic gate transformations, it’s universal enough to be used in a general way, which is nice. The official documentation does not really address this possibility.

What does the KiCAD “De Morgan” functionality actually do?

It lets you have two graphics for the same symbol. This is really useful for certain devices.

Here are a couple of examples:

The analog switch SPDT symbol should always show the “NC” state. But in one case, the control line is asserted high, in the other low.

The opamp inputs can be swapped, but the power (and other) pins stay in place.

Lots of other possiilities.

The standard solution would be to have two library symbols, which inflates your symbol library list and can complicate your BOM. If you’re fine with that, read no further.

How to create a second/alternate graphic for a library symbol?

This requires that the symbol to be modified is in your Personal Symbol Library!

Open the Symbol Editor and select the symbol in question. Let’s take the LM741 that a lot of people still seem to use.

Right-click in the graphics window, select “Symbol Properties” and tick “Has alternate body style (De Morgan)”; click “OK”:

The AND/OR buttons at the top of the window become active and are used to switch between your two graphics:

The original symbol is intact and will stay, but clicking the OR button will take you to the alternate symbol. You’ll see that it contains the pins, but no graphics. No problem, go back to the original symbol (AND button), copy the graphic, press the OR button and paste it.

Last, swap the input pins in the alternate symbol. Save. Done.

You now have two graphics for the same symbol, in this case an LM741 with regular/swapped input pins as shown above.

More advanced uses are possible, regular/alternate symbols are completely independent and can be drawn freely. Here’s a final example with two different graphics for the same counter symbol:

Using Alternate Symbols in practice

Add symbols to your schematic as usual. For the symbol(s) where you want to use the alternate graphic, right-click the symbol, select “Properties” and tick “Alternate symbol (De Morgan)”.
Using alternate symbols has no side-effects in other parts of KiCAD, eg, footprints, PCB layout or simulation.

Special issues

You may encounter symbols with “locked pins” in the Symbol Editor, though this is the exception. The symptom is:
When modifying/moving a pin in the alternate symbol, the pin is also changed in the regular symbol. Highly undesirable, but easy to solve.

Go to the regular symbol (AND button).
Right-click the problematic pin, select “Properties” and untick “Common to all body styles (De Morgan)”:


The pin will disappear from the alternate symbol, letting you add a pin of your choice. This can only be done on a pin-by-pin basis, multiple pin selection is not possible.