In all cases and for all purposes leave the original files intact or create safe backups.
Recently somebody had some problems with project migration from v4 to v7: [SOLVED] So disappointed.with Kicad. (EDIT: there’s much empty talk there, but also some useful tips, especially about new DRC warnings which may confuse those who haven’t used v7.)
One of the biggest changes was the total change of file formats of symbols and schematics between v5 and v6. Otherwise KiCad has small file format changes between major releases so that the older KiCad can’t use the newer files but in theory newer KiCad can always open older files. Sometimes there are changes which require manual inspection and maybe small changes to a migrated project, but I don’t remember this in other than layout. For example zone filling, clearance check and other algorithms may have changed a bit which may cause some DRC problem in some edge cases.
KiCad has a command line program kicad-cli. It has an option to upgrade an older library (or file in case of footprint, I don’t know) to the current KiCad version. This can be used to migrate libraries in batch. Otherwise you can add the old libraries normally to a newer KiCad, open each library in the library editor and save it back.
For projects you have to open the project and open/save the schematic and the PCB. For the schematic this means explicitly accepting the migration to the newer file format. For this schematic migration to work you have to have sym-lib-cache file existing in the project. Otherwise you will get boxes with question marks and you have to replace all symbols in some other way.
This will get you pretty far. I suggest you just try with adding (a copy of) your old library to a new fresh installation, see how it goes and then try migrating a project. You can ask further questions here.
Still one thing: after the migration both the schematic and the PCB will have old symbols and footprints inside them. When you continue to edit the project you have to decide if you want to leave those existing items as they are, and whether to change to new KiCad libraries – if you use KiCad’s libraries – for newly added items. In KiCad libraries the old symbol libraries are mostly compatible with new libraries because only pin locations are important, so you can update all symbols to use the latest KiCad library if you want to. The situation is different with footprints because all copper changes and also some other changes can potentially affect the layout. You can either update the footprints on the board and fix the problems, or leave the old footprints as they are and use new footprints for new items when you continue with the project.