Upgrade from V5 to V8 -- Symbols & Footprints

I started a project in June 2021 and released it to PCB. I loved Kicad – intuitive and sophisticated software. The project was put on hold and I recently picked it back up. I uninstalled (v5.1.10?) and installed V8.1. Everything looked great. I made changes to the schematic and PCB and even sent a preliminary package off for a quote. Then I ran a DRC and realized my libraries were hopeless. I’ve tried SO many things and nothing seems to work. Online documents talk about navigating from v4 to v5, from v5 to v7. Rescue libraries, on and on. I wish I had a definitive answer on what to do. I want to fix errors and warnings; I’m unwilling to simply “Exclude” issues. I’m happy to replace parts that are easy, like using Digikey’s new 0805’s (rounded corners – great!) but I don’t want to start over with the symbols I painstakingly made – especially when they’re RIGHT THERE and look great! Ugh! In Schematic Editor and in PCB Editor, the warnings are the same:
“Warning: The current configuration does not include the library …”
I’ve tried MANY things. What will actually work? Thanks!

These days, most of the native KiCad footprints have rounded corners on their pads.

Can you explain what your problem is? You write a lot about history / background, but the only part description of your problem is:

The days of “rescuing” KiCad projects are over. Both the [Project]-cache.lib and the [Project]-rescue.lib libraries were a thing in KiCad V5 only. Starting from V6, the information in those files is saved inside the schematic file itself.

Updating your projects / libraries one KiCad version at a time is a waste of time. KiCad V8 should be able to use older libraries directly. I think the rescue library is an ordinary library just like any other, but I’m less sure about the cache library. So you can just add the rescue library to the library table (With … / Preferences / Manage Symbol Libraries) If the library is in an older KiCad format, then you can migrate the format of such a library from the library management table.

Because the info from those libraries are duplicated inside the schematic and PCB files, you can also export them with: Schematic Editor / File / Export / Symbols to (new) Library and PCB Editor / File / Export / Footprints to (new) Library.

1 Like

For me it sounds like your symbols or footprints are linked to KiCad V5 libraries that were deleted when you uninstalled V5.
I’m not familiar with that as I use only my own libraries and they are not deleted when uninstalling old KiCad version and installing new so symbols and footprints at my schematic are linked to elements in my libraries that I made when KiCad was V4 and modified later.

So, what is on the dots?
Sometimes it’s difficult to recognize a misspelled name. Verify the library name is spelled correctly, and is actual in the location that KiCad expects to find it.

Thanks. Export Symbols/Footprints really fixed it. I’ve never seen any reference to that in any videos or discussions but … wow did it work! It just silenced everything but meaningful errors & warnings. Not 100% sure what exactly happened but I feel like I’m moving again!

These export functions create new libraries, and (optionally) update the links in the schematic and PCB files to point to the symbols and footprints in those libraries. Those new libraries only contain parts that are actually used in your project. They do not have all the parts that you created in your own / old libraries. To keep on using those, you still have to add those old libraries to the library tables.