I have a large schematic that, due to physical constraints, I have to split it up into 3 separate boards. I WANT to use 1 schematic file to link to all 3 PCB files simply because it will make my life easier. I need the reference designators to continue to count up across all 3 boards (not reset to R1, D1, etc. with each new board).
I have 2 solutions, but I don’t particularly like either. One is to copy/paste the part of the schematic relevant to each board into its own project file. The other is to put multiple boards into 1 pcb file. I am currently using the first solution, but it has been annoying to make any edits to one and them updating the part numbers across multiple files.
Is there any way I can do exactly what I want? Maybe I need to use hierarchical sheets or something?
KiCad is one PCB per project, hierarchical schematics will usually cause many DRC errors due to the same net name appearing on different boards. Managing a few related projects is easier than you think as in the link above.
It is easy to annotate each board R10XY, R20XY etc.
Then if you need to add a component later, and you will, it doesn’t shift the numbering of the other boards
This is in Annotate Schematic - Numbering - Use first free number after options
Develop the schematic as usual in a top project, but put each board’s section in a child sheet. There is an annotation option to prefix the refdes with the sheet number. But it doesn’t matter even if you use global annotation, they will be unique. This project will not be progressed to a PCB.
In 3 other projects, instantiate each child sheet from the top project using an extra-project path, e.g. ../topproject/child_sheet1.kicad_sch. Generate a PCB in each project and fabricate.
Edit the schematic from the top project only, but generate the PCBs in the subprojects.