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?
Easy make 1 or more new pages/sheets.
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:
Schematic Editor / Tools / Update PCB from Schematics [F8] to ensure they’re bot up to date.
Make a selection.
Cut [Ctrl + x] it out of the sheet.
Go to another sheet.
Schematic Editor / Edit / Paste Special (Or Paste special from the RMB popup menu).
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.
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
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.