Renumbering components on finished PCB

So finally a PCB is finished, but the order/numbering of the components on the PCB does not "look “good”; I want the numbering running in order like R1, R2, R3, R4, in rows/columns etc in a decided pattern.

In eagle I run a ULP (user language program) to make this thing, simple and always with good results. When I run the Tools/Geographical Annotate in KiCad (which I think should do about the same) it messes all up (=PCB is all out of order/ratnest light upp everywhere) after I run Tools/Update Schematics From PCB . What am I doing wrong? Is there instructions somewhere how to make this work, without needing to start from scratch with the routing of the PCB?

all steps in pcb-editor:
1.) Update pcb from schematic (to get both files consistent)
2.) Tools/Geographical Annotate
3.) feed back the new reference-annotation to the schematic:
Tools–>Update schematic from pcb.
There is a checkbox named: re-link footprints to schematic symbols based on their refrence designators.
As you have deliberatly changed the reference-designators: uncheck the checkbox.
The assignment will take place on the basis of the internal UUID-numbers every symbol+footprint has got
4.) to be sure I repeat step 1) to get the consistency back/forth between schematic/pcb. This is maybe not necessary.
5.) save both files

I got screwed up by this, too. (Hopefully you saved your design somewhere before running the tool, or better, you have it in a version-control repository!)

In the Update Schematics From PCB dialog, make sure that “Re-link footprints …” is NOT checked, and that all of the other options ARE checked.

The default is “Re-link footprints …” checked, and that breaks the design.

1 Like

Thanks a lot, now after trying your steps it works, though still a lot more steps compared to Eagle, which has Auto Annotation…

Btw, what is “version-control repository!”? I guess this means the automated backup zip files?

This once again leads to another important topic: Let’s develop “Save As” (or Save Ass)!

This is worth raising as an issue on the bug tracker.
What is this option for?

I agree with that, so I had a look at gitlab. There already is an issue very similar to it:

If the PCB has been changed for example by adding footprints to it, then there is no match between any (also manually added?) schematic symbol (yet), then you use this to connect schematic symbols to PCB footprints. It is the (only?) way to fix mis matches between the schematic and the PCB, as the UUID’s that KiCad normally uses for this are not user editable. I have used this occasionaly to “fix” things. It also makes it symmetric because PCB Editor / Tools / Update PCB from Schematic [F8] has the equivalent checkbox.

I added my “I have this issue too” two cents to the Gitlab issue.