That is our approach. (See the libs under the obsolete folder)
Not quite true. If you want to keep a uniform quality standard you will need to maintain even these symbols and footprints.
Just because something is used more often does not really make it more valuable. We librarians do not really care about what is used. We care about what we need or what we are interested in. (You know we are volunteers. We do this stuff because we find it interesting. If you want to change that you will need to pay us.)
I see this even a bit dangerous. If we collect such data we fall under GDPR and other rules about privacy. (A lot more work for basically no improve in library quality.)
I also think it would discourage users from submitting esoteric devices. (These are the ones that really make a library special. They test out the set of rules for the lib. They are interesting to check and therefore motivate the maintainers.)
You might not like it but the official library cares a lot more about quality than quantity. (We will never except anything below our strict standards. The staging area of parts that do not fulfill our standards are the open pull requests. We do not need a “unchecked community library” as it only adds more work for us maintainers. We are not prepared to clean up the work of others. If the contributor does not fix their component to meet our standards it will most likely die in the staging area.)
This is especially noticable when you compare the v4 lib to the v5 lib. We did not transfer everything over. A lot of stuff was too low quality so we did not include it in the new lib. (Especially for 3d models. If a model is not designed in a mechanical environment, it is not included in the v5 lib. But also some footprints and symbols did not make the cut as we could not find datasheets to check them against.)
Decentralize in this case seem to work for me, isolate my project from the library change as I needed. At the same time, I can pick new footprint from the KiCad public, or contribute when I found it missing one. Also allow a light way to capture my whole design in a repository without any outside dependency.
This tool also very helpfull: https://www.compuphase.com/electronics/kicadlibrarian_en.htm
@zoonman, I think @SembazuruCDE approach with some tune, + @GyrosGeier special connector symbol (with no specify type pins) in all 3 boards, the ERC may just work for multi boards check. But for the BOM, I think you make see the references difference when open individual boards project vs. multi-board one. There is a trick you can make them the same, but need write some script for that. That is up to your time and energy.
The issue with one schematic (showing all connections) is that it will try and MAKE that board, with all the connections, no matter how you try and split it up. worthless in practice.
I make this kind of multi-board system all the time, and each board is its own drawing and design, then I do a system level connection drawing (no PCB involved) tying them together. alignment is just a simple matter of noting board index points and key connector pins.
it is possible to make three schematics in a single drawing (no drawn connections) and result in 3 physical boards (snap apart style). duck soup.
you could even show connections with dotted lines (not tracks) if required for clarity.
To Zoonman and all others. I refer you to ANSI/Y14.44, Fig. 3 “Reference Designation in a Typical Diagram” as an example of a top level, overall schematic diagram of an equipment (“set”). First of all you need to assign reference designation prefixes using Y14.44, Fig. 7 “Typical System Subdivision” as a reference. For instance:
A1 for PBA1 (PBA is printed board assembly–IPC definition)
A2 for PBA2
A3 for PBA3
Those parts that are part of the enclosure, case, or chassis would have no ref des prefix.
Fig. 3 shows the use of the mechanical-boundary line (long-short-short-long, short-short-long, etc.) surrounding the circuitry that makes up the particular assembly or subassembly. The ref des prefix assigned is shown outside the mechanical-boundary line box in the upper left corner. However, I know of no schematic capture program, including KiCad, that recognizes this setup. What you need to do is use the ref des prefix that applies to each basic ref des. You would have an A1R1, A2R1, A3R1, A1C1, A2C1, A3C1, etc. This will give you a complete parts list (PL) ordered IAW the ref des prefix. If the overall schematic diagram is too large for one sheet you can have multiple sheets. In your case sheet 1 could be PBA1, sheet 2 could be PBA2, and sheet 3 could be PBA3, or however you would want to partition it.
For a single board design that can be broken apart to give separate boards, either mouse bites or the V-groove method can be used.
If you want three separate boards you can copy the schematic diagram and delete all parts not pertaining to the PBA you want. You could also delete the ref des prefix.
Assignment of reference designations for the connectors between the PBAs will depend on how you provision the setup. Let’s say you have PBA1 (A1) on top, PBA2 (A2) in the middle, and PBA3 (A3) on the bottom of your sandwich. Are you going to plug A2 into A3 and then A1 into A2 or are you going to plug A3 into A2 and then plug A1 into A2? You have to remember the most fixed, most movable rule and the class letter for a socket is X.
Hope this helps. If you have questions or need further explanation, just ask.