KiCad does not care where you put your libs. As long as it has read access to the place. Even keeping them inside a .pretty folder should work. But i would not really recommend it as .pretty denotes the footprint library and should hold .kicad_mod footprint files.
Tested it in 5.1.2 under windows. Meaning you might have a different root problem.
But kicad will not automatically add them to the tables no whether where you place them. You always need to use the library managers to do it. A very detailed writeup about library management (focusing on the word management rather than “adding libs to kicad”) is found in Library management in KiCad version 5
The .lib/dcm pairs are already your libraries.
In general if you get question marks than two problems are at play. You lost the cache lib or it is damaged and the symbol is not found under the name referenced. The reference consists (since version 5) of the pair “library nickname”:“symbol name” which means if either of these two changed in the lib then kicad can not find the symbol there.
The cache lib file is a special file found in the project directory. It has the name “project name”-cache.lib. That file should have an entry for every symbol you used in the project. If a symbol is no longer found in the libs then kicad will prompt the rescue dialog where it tells you that a symbol is now only found in the library table. It asks if you want to rescue that symbol which will result in the symbol being copied from the cache lib to a newly created rescue lib and all references will be updated to the new lib. The rescue lib is then added to the local library table.
If both the cache lib and original lib are missing then no dialog will appear and you get a question mark. (The most you can get is a message that a library file is not found but that would only come up if your lib tables are setup and you delete a file afterwards not if the library has changed name for example)
are they really .mod or .kicad_mod. .mod is from at least two major versions ago. (version 4 used .kicad_mod files per footprint in a library directory with .pretty entry)
Where you on version 4 or older before? You might run into trouble because you did not properly transfer your projects over. This might help Converting KiCad version 4 projects to version 5 (Remap a project)