I came across this strange behavior when moving components to a hierarchical sheet, then updating the PCB: the components are “re-added” and moved from their positions if there’s a layout already in place. If I lock them, they’re just added as duplicates.
When I moved them I cut them and then paste special - keep existing reference designators…
1 Like
To understand (and overcome) this behaviour its necessary to understand the technical background. Kicad identifies all symbols/footprints with an internal UUID-number. The synchronization between schematic <–> board also happens (normally) with this UUID-numbers. The reference-number you see in schematic is only for the user (exception below).
If you copy/paste some symbols in schematic the pasted symbols get new UUID-numbers, different from the original (even if you cut/paste the symbols). So the connection to the already placed footprints (in board) is lost, because they where assigned to the old-symbol-UUID-numbers.
To overcome this the following workflow has to be used:
- first be sure to have schematic <–>board fully synchronized (run command “Tools–>Update board from schematic”)
- do your copy/paste/moving in the schematic. Use “paste special → keep existing refrences” (as you have done)
- with this copy-paste-action you have symbols/footprint-pairs with broken UUID-synchronization, but the Reference-designators are the same. So the next step can resynchronize also the UUID-numbers:
- Now run again the synchronization-command: “Tools–>Update board from schematic”. But this time set the checkbox “ReLink footprints to schematic symbols based on their refrence-designators”.
- This should get schematic<–>board again in synchronization, without deleting old and adding new footprints.
- Last step: run again the synchronization-command: “Tools–>Update board from schematic”. This time the checkbox should be unchecked (unchecked==standard). This ensures that on the next invocation of this dialog the checkbox is set to unchecked state (and you are not accidentally work with checkbox set).
6 Likes
Great, this was very well explained, thank you!
1 Like
That’s a great explanation. It makes sense from an internals view, but seems rather more complicated than it should be for the average user.
Does anyone know of a technical reason KiCad couldn’t preserve the UUID for the symbol when one is cut & pasted, just as it preserves the reference designator? Obviously there would need to be some limitations on this to avoid repeated pastes from reusing the UUID.
Maybe @craftyjon or someone else more familiar with the internals could weigh in?
1 Like
Because the link between the schematic and the pcb is path, not just UUID of the symbol. Path includes the sheet path. See Update PCB from Schematic's match methods - #2 by eelik.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.