Ah, I think I know what you did - blame the bad UI design.
It will be a non-issue once the Devs get to refurbish EEschema, which is next on their agenda… PCBnew got the treatment already. But we’re probably months away from changes.
You added a new library by using the upper [Add] button, but didn’t get the path known to EEschema in the user-path-interface below that one (where there is another [Add] button).
This is the proper way:
- Remove the ‘WRONG’ labeled entry in your dialog (naturally a different lib/path than what you see in the pic)
- click on the [Add] button that is circled in red
- navigate to the path where your lib resides and chose either relative or absolute (I use absolute as relative had problems a while ago)
- click on the [Add] button at the top that is circled in blue
- navigate to the library file in question and add it
You could also edit the files manually, which would mean to remove C:/Program Files/KiCad402/share/kicad/library/ from LibName45 and LibName46 entries and placing it behind LibDir like so:
LibDir=C:/Program Files/KiCad402/share/kicad/library
The projects .pro file would then look like this for the symbol lib entries:
…
LibName43=relay_dpco
LibName44=relays (2)
LibName45=power_modif
LibName46=Power_Management
Same goes for the pcbnew section. Remove the path part from the lib entry and put it behind the LibDir above the footprint libs.
PS: if you want those custom symbol libs loaded/be set up when you create a new project you just have to do the same modifications to the kicad.pro file in the template folder (the one you posted first).
For pcbnew the ‘global’ library settings file that is used for project creation is located in a file called fp-lib-table instead of kicad.pro (KiCAD is in the middle of changes, so just accept this how it is at the moment).
Location:
C:\Users\JonDoe\AppData\Roaming\kicad
PPS: Next non-obvious obstacle to eeschema libs:
the order of libs in the upper window is important if you got symbols with the same name in libraries… KiCAD will ALWAYS chose the symbol from the lib that’s highest in that list, no matter what you chose during placement.
So if you got a GND symbol in power_modif lib and there is a GND symbol in power lib and you are going to place the GND symbol from power_modif in EEschema… the one from power will be used instead of power_modif, as power is #2 and power_modif is #45.
That’s why there are [Up] and [Down] buttons there… tip: click it once (get it focused) and then press down [ENTER], makes moving entries up/down faster than clicking with the Mouse 
PPPS: same stuff happens when you load a project with different symbols from the ones you have currently set up… EEschema will offer to rescue them… remember it when you encounter it, don’t stress about it for now (just don’t save the schematic when something happens you don’t like).