The scheme I normally use with Altium libraries is:
Library part name: type-size-value
e.g. Resistor 0805 10.0k 1%
Connector DB9 <MfgPN>
etc.
The parts are well drawn (I'm picky!), in consistent sizes and styles, using Altium's traditional piss yellow background for ICs (rectangles with pins coming out, or shapes like op-amps), or light blue for "active" discretes (the circles of transistors, etc.). The data includes a recommended Supplier Link (Supplier/PN, Mfg/PN, and additional parameters if ever needed). If the part is a passive (resistor, etc.), it has a Value parameter which is displayed as a label. Otherwise, the Comment field is used, carrying a truncated MfgPN by default (but this is recommended to be changed to something descriptive when needed, e.g. for named connectors).
Footprints I'm a bit more lax on naming convention; if it's general, I use the common name, or something descriptive (e.g., CAPAE63X70, SOIC-8, HDR2X10_SMT_50MIL). If it's part-specific, I use MfgPN (e.g., connectors most often).
I also try to locate useful, accurate, good looking 3D models (e.g. from 3D ContentCentral, or there's another I can't remember; I suggest creating a slightly bogus login, since they just want to sell you stuff... or your info), and use those in the footprints.
I avoid using multiple footprint options for a given component.
The advice given above is good; a common library which grows carefully is probably the best. Only add parts when they are consistent with the above rules (or whatever variation of them you might have for your workplace), and try to avoid removing or renaming parts, except also by careful review. (When I'm working alone, I have a sense of which footprints and parts I've already used, and which ones can still be renamed or modified. This decision gets exponentially more complicated for more users, so tread carefully.)
Tim