I’ve been given a KiCad project created on Mac in version 8.0.0 to modify. If I open the schematic in version 9.0.2 on Ubuntu, the reference designators for all symbols are unassigned and appear as “R?,” “U?,” etc. I’ve confirmed with the sender that we have the same set of project files, and that when they open the project on their Mac in version 8, the reference designators show up as they expect.
Oddly, if I open the .kicad_sch file in a text editor, the reference designators seem to be present under the “property ‘Reference’” entry for each symbol, but they don’t show up when opening the file in the schematic editor. I tried opening the files in version 8.0.7 on a Windows 10 machine, but I’m seeing the same behavior.
Any thoughts as to what might be happening here? Unfortunately I’m not able to share the files, but I’ve attached a screenshot of part of the .kicad_sch file in a text editor showing that one of the capacitors has a ref des listed. This has never happened to me when migrating my personal projects from v8 to v9, so I’m a little puzzled.
How are you opening the file?
If you open the .kicad_sch directly, this is a typical problem.
You need to open the .kicad_pro file and take it from there.
Thanks for your replies. I think I may have found a solution, which I’ll detail in the next paragraph. In answer to your questions, opening the schematic in 8.0.7 first then saving it and re-opening it in 9.0.2 did not work, and looking in a text editor I see that the ref designators which were there get replaced with their unassigned versions (R?, U?, etc). I also tried opening the schematic via the .kicad_pro file and that made no difference.
Here’s what I did that seems to have restored the existing ref designators:
First I made a copy of the original .kicad_sch file, then opened that copy in 8.0.7 and saved it.
Then I opened the original and new .kicad_sch file in notepad++ and used the compare plugin to highlight all differences. Aside from the ref designators getting reset, the other main difference is that the instances “path” string is different (see attached picture).
I wrote down the path string from the saved copy of the schematic, then did a find-and-replace operation in the original schematic to replace the original path with the new one.
After doing that, the original schematic opens up in both 8.0.7 and 9.0.2 with the original reference designator numbers in-tact. Not sure what caused this, but I suspect there’s something weird about how the original designer was storing/organizing their project files. Whether or not they’ll have this same issue when I send the modified files back to them remains to be seen.
