Designing a PCB with variable-sized component alternatives

Question

I'd like to get a little PCB manufactured with a basic circuit that I can populate with components of various sizes. E.g. have a place where any of a range of possible capacitor sizes could go. So I would have a chain of leads, like this, for example, where depending on size, I would use a closer or further-apart lead for the component in question:

---O-O-O O---

I'm finding it difficult to convince KiCad or Fritzing to let me do that. They seem to think that any component has exacly one size, and I can't find an "empty lead" part to add either.

Any advice how to best go about this?

Answer 1

I make double and triple footprints in KiCAD quite regularly and it works out quite well. You need to be careful about production constraints (avoid holes in SMD pads, etc), but KiCAD does allow you to do what you want.

There are several ways to go about it:

• Superpose all the footprints one on top of the other. You need to ignore the specific DRC errors about overlapping courtyards, and sometimes place holes very precisely in the same location.
• Create a specific footprint. In your example, you would give the same PAD index number for a group of PADs. Once you do your PCB layout, the router will request you to add the traces between the PADs that have the same indexes. So you still have some freedom on how you want to route this.

Here is an example where I superpose two different rectifying bridges. The center is slightly different so that the PADs do not superpose:

Here is an example where I can put one out of two fuse holders using a single footprint:

And another case where I superposed two RJ45 connectors - one SMD and one THT - the "holes" are superposed:

Answer 2

while I remember there being a few more flexible footprints (especially, the "hand soldering" SMD footprints), this simply screams "you want something oddly specific, so, go and design your own footprint". It's surprisingly easy!

If you want, you can also do the nice FOSS thing and then upstream your new footprint to the kicad-library.

Answer 3

I generally would not suggest combining multiple components into one footprint/symbol. This will hide a lot of information from a reader of the schematic. It is much better to have one symbol per possible alternative in the schematic (connected in parallel). This allows you to create a BOM for every variation as required. (This could lead to false positive ERC errors/warnings depending on how the symbols are designed. Sadly there is no "do not show this one message in the future" option in KiCad.)

You can then overlap the footprints as needed in pcbnew, but make sure not to overlap pads as this can create trouble with soldering. There simply is a tradeoff between component selection flexibility and board size. (This restriction also applies when making a single footprint for all possible components.)

Another benefit to having one symbol/footprint per possible combination is that you are still get one centroid per possible part in the pos file which is required for automated manufacturing. Meaning combining different options within a footprint will likely restrict your options for automated manufacturing. (You never know if you might not in some future want to go this route for some of your projects.)

Answer 4

You could do this in Fritzing using a 1 x n pin header component to add the n extra holes (a 1-pin header is your 'empty lead component'). Place the header on the PCB layout first, place the copper tracks as you want them, then go back to the schematic view and tidy up there. You'll probably want to hide the silkscreen for the header.

This won't leave you with a fully professional looking schematic, but if you needed that you wouldn't be using Fritzing. It should achieve what you need on the PCB though.