The KiCAD Symbol Library contains many multi-unit symbols. The simplest way to visualize units is to think about something like a quad op-amp, eg, LM324 as the symbol, and each of the four op-amps as units (A, B, C, D).
Important to know is that the units do not need to be the same!
As always, creating or editing symbols is only possible in your personal libraries, the standard libraries supplied with KiCAD are read-only. More information in this FAQ:
Additionally, it’s a very good idea to keep the KLC (KiCAD Library Conventions) open in a browser tab/window when creating a new symbol. Then you have a reference when in doubt:
This FAQ will mainly focus on creating KLC-conformant symbols. An Appendix shows other options.
There are two basic ways of creating multi-unit symbols:
1: copy an existing standard library symbol to your personal library and modify it (this is the easiest way).
2: create a new multi-unit symbol from scratch (this FAQ).
Creation From Scratch
This example creates a new symbol called “74HC1234” containing four XNOR gates (yeah, yeah, I know…).
Before you do anything at all, set your grid to 50 mils.
From the KiCAD Welcome/Main screen, open the Symbol Editor and select the library that you want to add your new symbol/part to (in this case, “0_74xx”). Click the “New Symbol” icon or use the File menu. You’ll get this dialog box:
The only thing you need to do here is to enter the new symbol name: “74HC1234”, then click OK. The rest can be done later.
This brings up the library list again, this time with the addition of the new part in the list, and the new part open for editing.
Select the “Displays symbol properties dialog” icon, or simply right-click in the white space in the editor screen and select “Symbol properties…”.
You’ll be taken to this screen, which is the standard one for editing symbol properties:
In green you see the information inherited from the previous dialog. In yellow, you should change the “Value” field to “74HC1234” (this will be shown when the symbol is used on the schematic) and the “Description” to something like “XNOR, 2-Input, Quad” (this is visible in the symbol library list).
The fields in red are the interesting ones.
Set “Number of units” to 5 (yes, it’s a quad gate. But the fifth unit will be needed later. We’ll see why).
Untick all three tick boxes in the red field.
Save by clicking OK. You’ll be returned to the Symbol Editor, and your new symbol and the “Unit” field is now active:
Select “Unit A” and draw your symbol and add signal pins as appropriate (input, output; line, inverted etc.). Don’t assign pin numbers:
Select the symbol graphic including its pins and do a simple copy/paste to Units B, C and D. All four units (A, B, C, D) should now look the same.
The Fifth Unit
The fifth unit (Unit E) is needed for power connections to the new symbol. It’s is simply a rectangular graphic with power pins attached. Most KiCAD libraries use a 400(X) by 600(Y) mils size, but you can make it any shape and size you like.
Simply add a pin at the top and at the bottom of the rectangle, and define each pin as “Power input”. Name them according to the device (eg, VCC/VDD and GND/VEE/VSS etc.).
The only thing remaining is adding pin numbers, which is done by clicking the “Pin Table” icon and entering the pin numbers in the table:
Finally, adding the units to your schematic will look like this:
Final Comments
This might look involved, but creating a multi-unit symbol takes less than 5 minutes. Even less if you copy and modify an existing symbol from the standard or personal library.
Appendix:
Non-KLC-Conformant Multi-Unit Symbols
Every designer/company has own styles and rules for libraries. Schematic symbols without a separate power unit might be more desirable, like these:
Variant 1:
This has power connections to each unit of the symbol (with or without pin name). It does complicate the schematic, though.
Variant 2:
This connects power to just one of the units (normally A) and is neater in the schematic.
For both variants, proceed as in the main FAQ, but in the Symbol Properties screen set “Number of Units” to 4.
The tick box “Show pin name” defines the difference between U1 and U2.
Variant 1:
Create unit A and add power pins to it. Copy and paste to units B, C, D and finalize by adding the pin numbers using the “Pin Table” function.
You’ll now have a multi-unit symbol as in the Variant 1 screenshot.
Variant 2 is very similar.
Do exactly as with Variant 1, but don’t add the power pins. Do the copy/paste to B, C, D first, and then add the power pins to unit A. Assign the pin numbers.
Save, and all’s complete, both should look like the screenshots above.