Move parts of schematics to new pages

I’ve seen this topic discussed a few times here (more older threads) and now with version 5.99 I wonder is it possible to simple move selected parts of a schematics to new pages?

  1. Easy make 1 or more new pages/sheets.
  2. Move selected parts of the schematics to the new pages – without loosing the connection references to the PCB (annotation) in a case where the PCB may be already completed.

It’s one of the many many enhancements in KiCad-nightly V5.99, although I admit the method can still be improved.

The way it works:

  1. Schematic Editor / Tools / Update PCB from Schematics [F8] to ensure they’re bot up to date.
  2. Make a selection.
  3. Cut [Ctrl + x] it out of the sheet.
  4. Go to another sheet.
  5. Schematic Editor / Edit / Paste Special (Or Paste special from the RMB popup menu).
  6. Make sure to select: Keep existing reference designators, even if they are duplicated
    • This preserves the RefDes, but it does assign new UUID’s to the pasted symbols.
    • This has to be fixed, and that is why it started in 1). with updating the PCB.
  7. Schematic Editor / Tools / Update PCB from Schematics [F8] and make sure to select: Options / Re-link footprints to schematic symbols based on their reference designators
1 Like

Alas, I can’t edit my old follow-up to a FAQ article to add this use case there, but I hope there will appear a visible link to this thread.

Thanks paul. It worked well (after I figured out how to add the new, blank pages). It’s some more work compared to Eagle but it should be possible to practice & learn.

Try now. It seems the first post in a topic is automatically a WIKI page but not follow up posts.

1 Like