How to show a NPN transistor with 2 Collectors

I am working with a 4 NPN SMD chip, FFB2222A / FMB2222A / MMPQ2222A, and I want to make a symbol that has 4 separate NPN transistors to make it easier to visualize on the schematic. Each NPN transistor in the package has 2 pins for the collector, connected together as shown in this diagram from the datasheet.
Screenshot from 2024-05-07 07-07-39
pin 1 = C1

Here what I have so far for the symbol for the chip (ignore the resistors, just checking that all the pins are connected correctly on the pcb.)

With what I have, I cannot connect a trace to pins 2,4,6, and 8 on the pcb.

What would be the best way to show the additional collector pins (i.e. pins 2,4,6, and 8) and the internal connections?

There are at least 3 options.

  1. You can modify your schematic symbol and use “pin stacking”. This is for example used in the CSD16301Q2 in KiCad’s default libraries. I don’t like pin stacking myself.
  2. You can modify your schematic symbol and just draw the pins. Sometimes you see power mosfets with 3 or more source and drain pins on a schematic. The advantage of this is that you can find all pin numbers on the schematic if the PCB needs repair. (Edit: This is what gmc posted below).
  3. You can modify the the footprint and rename some pads. If pads have the same pad number, KiCad assumes they all have to be connected, so if you renumber pad No 2 to 1, then you can simply draw a track between them.

You can modify the darlington symbol and customize it for your purpose.

The symbol editor is really easy to use and everyone needs to learn it. This just took a few minutes.

testlib.kicad_sym (14.0 KB)

You can download the symbol and footprint from this site.

I want individual NPN transistors to make the schematic easier to read and understand.

This is the symbol available for download, and I find wiring it up and checking cumbersome versus individual NPN transistors.

Screenshot from 2024-05-07 11-56-56

This is easier for me to understand and visually check.

To each his/her own!

And yes, the symbol editor is easy to use once one has used it!

Then you can make a four-part symbol with A,B,C,D sections for each transistor (and no power section). Look how it is done for dual or quad opamps, for example.

If you look at the screenshot in the opening post, you see it has already got a symbol with four units.
This “drawing a symbol” deviation surprises me a bit, because the only question here was about the pin numbering, and matching with a footprint.

Well, fair enough. Here’s a separate one – just edit symbol properties to add wherever your local soic16-150mil footprint resides:

testlib2.kicad_sym (20.1 KB)

While the circuit will work with the pins open, it is better to connect them for power dissipation