Create a single footprint for 2 components

[MicGus]

Hello,
I want to create a single footprint for 2 components.
In an assembly I want to have on a single PCB the possibility of mounting a rectilinear potentiometer of 2 different sizes.
One of the potentiometers is 45mm and the other 60mm.
I tried and it seems to work, but I have errors when checking with “Design rule checking”
I use the symbol “Device:R_Potentiometer_US”

Is there a solution or should I live as with.?

Thanks in advance for your answers

[Piotr]

I suppose that 1bis (and 2bis) should simply be 1 and 2.
Kicad will need you to connect them at PCB.
You can also connect them directly in footprint, I think.

[retiredfeline]

I suppose you have combined the two footprints by pasting one into the other. You will get duplicated courtyards and create DRC errors. It’s better to take the longer footprint and add pads and mounting holes to it for the shorter component.

Here’s a footprint I made which suits either the rectangular or square active crystal oscillator cans. You see that I have chosen to duplicate pads 1 and 14. (I stuck with the original numbering of the DIP-14 package, so in the symbol I use pins 1, 7, 8 and 14.)

One thing I should have drawn is a silkscreen line indicating where the DIP-8 square part should be placed. Ok, just fixed that right away.

I probably should have added more indications like a paint dot next to pad 1 but this is a personal project and the footprint is only for myself.

[MicGus]

I connected them on the PCB

[paulvdh]

In KiCad, when a footprint has multiple pads with the same pad number, then KiCad simply assumes those pads always have to be connected to each other. That is the reason why the screenshot that retiredfeline posted works. It has two pad with pad number 1 and two pads with pad number 14. The schematic symbol does of course also needs these same pad numbers.

[MicGus]

Thanks for your answer
I took the footprint of a potentiometer to which I added 2 pads by copying pads 1 and 2.
Is this a mistake?
Do I have to create the pads from scratch?

[paulvdh]

@MicGus

Do I have to create the pads from scratch?

No, making a copy (or a duplicate) of a pad is just fine.

[MicGus]

Thanks for your answer
Great, it works, I didn’t dare use the same number on 2 pads.

[RaptorUK]

@MicGus

In an assembly I want to have on a single PCB the possibility of mounting a rectilinear potentiometer of 2 different sizes.

If you make one footprint you are going to give yourself issues with your BOM . . . I suggest you don’t do it the way you are suggesting. Use two footprints, set the one you don’t want to be “Do not populate” and “Exclude from bill of materials” and it will not be on the PCB and not in the BOM.

If you want to semi-automate the process look into a Plugin called KiVar

[jmk]

I’ve always included the tracks between the same named pads in the footprint.
Using the old cat’s example, the two 14s are joined with a track, as are the two 1s.

[Piotr]

@RaptorUK

If you make one footprint you are going to give yourself issues with your BOM . . .

Not necessarily…
Few years ago there were problems with HVD72 I use. They appeared and disappeared in different casings. Contract manufacturer suggested to make a footprint so he could use elements that are just accessible. So I made one footprint for SO8+SON8 packages. I write in BOM not one part for element but a list of parts I accept to be used (for example as alternative to LM25017 I list LM5017) so for this part I simply listed it in SO8 and in SON8 (even it seems being typical element there are no other manufacturer replacements for HVD72 to specify other element in SO8).

[MicGus]

Thanks everyone. Your answers helped me solve my problem.

[paulvdh]

Don’t mark your own post as the “solution”, but mark the post that is the best answer to the original question as the solution. The goal is to help people who are searching the forum for problems they have to guide them to answers quicker.

[retiredfeline]

@RaptorUK

I suggest you don’t do it the way you are suggesting. Use two footprints, set the one you don’t want to be “Do not populate” and “Exclude from bill of materials” and it will not be on the PCB and not in the BOM

That’s a different scenario where you manufacture different boards depending on which kind of part you have. Here you use the same footprint on all boards and place the part you have appropriately. It’s a similar story with this standard footprint in the KiCad library:

Strange CP_Radial footprint with two sets of pads

Could someone please have a look at this footprint in the v8 library: CP_Radial_D10.0mm_P2.50mm_P5.00mm and tell me why that pads are like this: [image] There are others in the library with two pitches. Is this one of those Frankenstein footprints meant to accommodate two pin pitches?

[retiredfeline]

@jmk

I’ve always included the tracks between the same named pads in the footprint.

One reason for delaying gratification is that for THT parts making that connection later gives you the flexibility of choosing the copper layer at layout time.

[RaptorUK]

@retiredfeline

That’s a different scenario where you manufacture different boards depending on which kind of part you have

Naaa, I was suggesting including both footprints but just populating one or the other . . . so just one PCB suitable for both variants of the component.