Schematic Symbol Pin Numbering - Multiple Numbering on Single Pin

[Antonio_Benci]

KiCAD Newby question, as I can’t seem to find a succinct answer.

Can a symbol pin contain more than one number.
I have a custom component layout that has 8 pins, 4 pairs of pins each pair is a duplicate function, eg

1,2 - VinNEG
3,4 - VinPOS
5,6 - VoutPOS
7,8 - VoutNEG

As I would like to draw a generic symbol with only four graphical pins, I would like to label each 1,2, etc.

Thanks.

[retiredfeline]

Use each number more than once, that’s allowed, say 1 1 2 2 3 3 4 4 or maybe 1 1 3 3 5 5 7 7. When routing, pads of the same number will belong to the same net. You can see this in a SPST tactile switch that has 4 pins for mechanical reasons.

[mf_ibfeew]

First I assume that you are talking about a generic symbol (4 pins) for an example footprint (8pads, which connect to the 4 pins)

As I would like to draw a generic symbol with only four graphical pins, I would like to label each 1,2, etc.

You can draw such a generic symbol, but than you have to draw special footprints for that

That is currently a little bit difficult and both possible options require a compromise.
You have the Kicad restrictions in mind:

• It’s not allowed to have mutiple symbol-pins with same pinnumbers
• It’s allowed to have multiple pads in the footprint with the same padnumber. All these pads are connected together at board-level (during routing). See answer above (retirefeline).
• the connection between schematic (symbol) and board (footprint) happens with pinnumber == padnumber.

So there are 2 options:

• draw a generic symbol with pins 1,2,3,4
  advantage: always same symbol can be used
  disadvantage: for most footprints you have to draw a specialized footprint. In your original example you can’t use a standard 8-pad-footprint, as these standard footprints would have pads 1…4 connected with your pins 1…4 and the other pads 5…8 would be unconnected.
• use generic footprints, but draw a special symbol for every different footprint / different footprint pin assignment
  advantage: use the standard footprint libraries
  disadvantage: custom symbols for different symbol<–>footprint combinations

So to use generic symbols as well as generic footprints is currently not possible.

remark: I don’t know if the database libraries offer a better/different solution to this task.

[eelik]

@mf_ibfeew

So there are 2 options:

Actually it’s possible to attach a 4-pin footprint to an 8-pin symbol. (To my surprise 7.99 doesn’t warn about that while updating the PCB from schematic, and it’s caught only when “Test for parity between PCB and schematic” is enabled in the DRC dialog where it belongs to Schematic Parity tab.) This would be a third option: one symbol with 8 pins and two different footprints for 4-pin and 8-pin versions where the first footprint has pads 1…4 and the second 1…8.