Created sub-sheets and lost assosiation to components on PCB!

[FriedMule]

Because my project got too cluttered did I chose to move via copy-past to sub-sheets but when I now go into PCBnew and press "load netlist" does pcbnew creates new footprints and it looks like the original and carefully placed footprints are no longer "connected" to those from the schematic.
Is there a way to correct that?

[marmelade]

I have observed this behaviour as well. This is because the designator-references are lost.

As far as I am aware of there is no automated process to re-align the designators with your pcb. Havn't tried it yet but manually "renaming" your components to the inital designator should still work (target: sch-netlist and pcb-netlist match each other). If this is a practical solution depends on how many components you have shoved on the new subsheet....

Maybe the KiCAD pros know of a better solution?

[Doctorandus_P]

Normally the syncronisation between the schematic and the PCB is maintained via "timestamp" vlaues (will change to: "UUID" in KiCad V6).

If you do a copy and paste schematic symbols this information is lost.
To repair this, you have to use the same RefDes values in the schematic as the old symbols, and then while updating the PCB use the function "Match Method / Re-associate footprints by reference"

Another way to fix it is to draw a short track segment from the attachment point of pin 1 of each old Footprint, then delete the old Footprints, grab the new one by pin 1 and move it to the endpoint of the track.

[poeschlr]

In version 5 you are basically left with only manual options or some direct file hacking. (As indicated by the others who were faster than me)

Version 6 will bring a paste special command that allows keeping the reference designators unchanged. With that you can then rebuild the connection to the PCB side of things.

[thinkfat]

When doing cut&paste from a sheet to a sub-sheet, your only hope is to maintain the reference values manually. Make a screenshot of the circuit you're moving and then annotate the part references manually so that they match their previous values. Then, when updating the PCB from the schematic, choose "Re-associate footprints by reference". KiCAD 6 will make this much easier with a "Paste Special" command.