Rename Reference on both Schematic and PCB

Schematic
1

Hi,
I have two finished schematic and PCB layout. Now I want to merge both layouts in single PCB as I want them to be connected and in single PCB only.

Problem is both Schematic is big and have R1 C1 U1 etc common. How can I change any one Schematic with say 100x all R C and U and so directly update it’s PCB layout with the same.

I do not want to modify layout of either design as I need them as it is layout.

2

I have not tested this, but I think this method will get you close:

  1. Create a new project (just to be safe)
  2. Copy both schematics, PCB’s and possibly custom libraries etc.
  3. Create the empty PCB file (probably already exists).
  4. Exit KiCad completely (also the project manager).
  5. Open Pcbnew directly (not from a project). This opens it in “standalone mode”.
  6. Pcbnew / File / Open -> The (empty) PCB of your new project.
  7. Pcbnew / File / Append Board -> One of the existing PCB layouts.
  8. Repeat 7). for the other PCB.
  9. Save & Exit Pcbnew.
  10. Start KiCad Project manager again and open schematic.
  11. In Eeschema, add 2 hierarchical sheets, and reuse the exiting schematic files.
  12. Clear the annotation in one of the schematics.
  13. Re-annotate the schematic, keep annotation for the other schematic.
  14. [F8] to update the Refdes values to Pcbnew.

Some notes:

  • This is untested, you may have some problems.
  • There can not be 2 different components with the same RefDes, so some renumbering is always needed.
  • Normally KiCad uses “Timestamps” to synchronize schematic symbols and PCB footprints. which means you can change the RefDes without loosing sync.
  • You may loose RefDes / Timestamp values when inserting the sheets in step 11. I’m not sure about those details.
  • If you get into trouble, then explain here. there probably are workarounds.
  • If you need more help, it helps if you zip the whole project and post it here.
1 Like
3

A way to get one of your board designs to reference designators other than your second one would be by use of the annotate schematic tool and the use “first free number after” option set to something higher than what is on your second design. You will of course need to select “reset, but keep order of multi unit parts” to get new references on an already annotated design.

After that update pcb from schematic with “by reference” selected as detailed in Update PCB from Schematic's match methods

Only after that would i try to combine the pcbs as you then at least have the refdes common which will make reconnection easier.

After you have successfully reconnected the combined schematic with the combined pcb you can again reanotate to your liking to get more reasonably refdes numbers than what you might have with the above process. (don’t forget to again update the pcb but now with “keep association”)

4

This looks good. Will try this and will give an update. Thank you.

5

Small addition:
I already wrote I did not test it.
Rene may well be right in changing the order of doing this a bit.

If you get into a situation which needs relatively much manual renaming to get through one of the steps and you’re not sure if it works, then it may be better to create a very simple test project to get the workflow right.

6

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.