I want to open an old Kicad project, and although I’m adding the required libraries to the project, Kicad doesn’t see them. What am I doing wrong, or what is Kicad doing wrong?
Kicad project from: GitHub - aventuri/DSP-ADAU1452-StandAlone: Open Hardware DSP Platform ADAU145x DSP supporting ADAU1452, ADAU1451, and ADAU1450 devices
I do not have the answers. But…do you know with what KiCad version this project was last edited?
I am pretty sure you can reach back to versions 6 or 7 but I do not know if you can go a lot earlier than that.
Wow, that project is really old, 10 years. The README says KiCad 4.
Also you are looking at a fork of the original project which is GitHub - ohdsp/DSP-ADAU1452: Open Hardware DSP Platform ADAU145x DSP supporting ADAU1452, ADAU1451, and ADAU1450 devices
But that still used KiCad 4.
I tried importing the indicated library (in the original project) and was able to add it as a Legacy library.
I didn’t migrate it to the current format as this was only a test.
Would it be difficult to have some online tools for migrating older KiCad files? Just a curious-idea.
I thinkt the migration succeeded but the nickname for the library in the schematic is not the same as the nickname assigned by the OP to the legacy library, so eeschema failed to find the symbols.
So there’s no way to open such an old project in KiCad? It’s a shame, though. It’s a very well-designed four-layer board, and now I’d have to start from scratch. I can’t even open the schematic! There should be some tool to migrate from the old version to the new one.
No, I think you can fix it.
Proceed by ignoring the not found errors. A lot of the symbols will show up as question marks in the schematic. Select one to edit the properties and note the nickname of the library, the part before the colon.
Then go into Manage Symbol libraries and make the imported library nickname the same as this. Pay attention to the case of letters.
Now reopen the schematic and see if it’s fixed.
Before you do this, make sure you can view the symbols in your imported library.
This is my best guess of what’s happening.
The problem is that I can’t open any schematics for any hierarchical parts. Kicad restarts when I try to open them. I don’t have any schematics with question marks instead of symbols. Try it yourself – I’m using version 9.0.3.
Sorry, I’m still on v8 so can’t help you there. If KiCad crashes, then that’s a bug.
Edit: Ok, I opened the project in v8, then added the MyKiCadLibs-Lib as a project specific library. When I opened the schematic I got a lot of ?? symbols.
The trick is to go to Tools > Edit Symbol Library Links and fix up all the orphan links to point to the imported MyKiCadLibs-Lib. There are a lot so it’s tedious, so I only did a few, but as you can see from this screenshot, some progress has been made.
You could also add MyKiCadLibs-Lib as a global personal library.
I think you have to do something similar with the footprint library.
Trying with 9.0.4rc1. Lots of complaints about two missing libraries and no cache files.
Then I can open the root schematic. Clicking on the PSU schematic box causes a crash.
The Project file browser does not show the subsheets.
Sounds like a regression bug between v8 and v9.
OP could do the migration with an Appimage v8.
Where did you find that library, it is not in the directory
There’s a link to the repo in the README.md file.
This happens to me, too. But KiCad doesn’t restart, it’s just closed (it crashes).
I found MyKicad… and added it to a clean copy of the directory.
Added it as a project specific library and the schematic opened - lots of boxes due to the still missing Power.lib, but that is easy to fix. No crashing.
This is why archiving old KiCad versions needs so many additional files or the cache. Modern KiCad caches the symbols and footprints in the files to prevent this.
There’s definitely a bug opening this old schematic in v9 and v10. I’ve got a trivial fix, but I want to check there’s nothing more fundamental we should fix before committing it.
No. Not true. This project definitely can be rescued. But like the others here, I’m also bumping into some difficulties.
I am still on KiCad V8 myself and also tinkered a bit.
I started with:
paul@cezanne:~$ git clone https://github.com/aventuri/DSP-ADAU1452-StandAlone.git
Cloning into 'DSP-ADAU1452-StandAlone'...
remote: Enumerating objects: 43, done.
remote: Total 43 (delta 0), reused 0 (delta 0), pack-reused 43 (from 1)
Unpacking objects: 100% (43/43), 2.48 MiB | 7.09 MiB/s, done.
paul@cezanne:~$ git clone https://github.com/ohdsp/KiCad-Libs.git
Cloning into 'KiCad-Libs'...
remote: Enumerating objects: 290, done.
remote: Total 290 (delta 0), reused 0 (delta 0), pack-reused 290 (from 1)
Receiving objects: 100% (290/290), 143.69 KiB | 2.87 MiB/s, done.
Resolving deltas: 100% (244/244), done.
I could not add the MyKiCadLibs-Lib.lib to the project normally. KiCad detects it as a legacy library, but for some reasons it seems to forget it, and even replaces it in the library table (I added it as a project specific library). After a bit of fiddling (copied the “MyKiCadLibs” to a “-cache.lib”, and also copied and moved it to the project directory and added it again as a library) I managed to rescue the project. After that I manually mapped the power symbols to KiCad native symbols. Now it looks like:
The other sheets also look quite good, The only issue I saw is with one connector, which has shifted. This is probably caused by using a slightly different library symbol.
And I had an annotation issue with (all or some?) multi unit symbols. Apparently KiCad did not recognize the units. Affected IC’s are: U404, U203, U401.
I agree that we should never get a crash. Complaining about being unable to do anything due to missing libraries is fine. This example is the most extreme that I have come across as even “R” and “C” are in that library.
This is the issue I’ve filed for this crash: eeschema crash navigating v4 schematic (#21497) · Issues · KiCad / KiCad Source Code / kicad · GitLab
I’m glad I helped find the bug in version 9.
On the other hand, why did you have to add each resistor and capacitor separately? Kicad didn’t recognize that they were all C and R? They only differed in values. But okay, done.
