Relative path for KiCad custom symbols

Question

I'm trying to make my KiCad projects portable & that requires my custom symbols & footprint I used for these different projects be portable as well. So I'm putting my "my_symbols" & "my_footprints" folders in the same level as the folders for each projects.

Now, for the projects to refer to these custom footprints I go to Preferences > Manage Footprint Libraries > Project Specific Libraries > [Browse Folder] & browse for my_footprint folder. When the absolute path is inserted in Library Path, I make it relative by overwriting "../my_footprints" & click OK. This seems to work as the footprints are available for adding, editing or updating.

The problem is doing the same for symbols. I go to Preferences > Manage Symbol Libraries > Project Specific Libraries > [Browse Folder] & browse for the individual kicad_syms I have. When the absolute path is inserted in Library Path I change it to "../my_symbols/xxxx.kicad_sym". This seemingly works as I click OK, but though the name of the symbol is in the list for adding or editing, selecting it yields nothing, "No symbols selected".

Sure I can simply import the symbols for the project every time I change folders or workstation, but there's gotta be a smoother way.

Answer 1

Symbol and footprint library paths can contain path variable references. They are shown in "Path substitutions" zone in Symbols/Footprint libraries dialog.

One of these variables is ${KIPRJMOD} which references the project directory. If you use path like ${KIPRJMOD}/my_symbols/Lib_Name.kicad_sym, your project will be portable.

You may also add global paths in Preferences -> Configure Paths in KiCAD project window. You may for instance define a path for checkout of a custom KiCAD library repository you use from multiple projects.

Note: IIRC, relative paths without ${KIPRJMOD} or other absolute reference are relative to current working directory of the KiCAD executable, which may sometimes work, but is totally useless for portability.