Conventional way to manage and use the libraries in Altium
Create a folder and name it "Altium Libraries" (or any other name you prefer). This folder will contain all your libraries. 
Within that folder create several subfolders with names like:
"Resistors" (for all resistors you will add to the resistors library),
"Capacitors" (for all capacitors you will add to the capacitors library), 
"Atmel" (for all parts from Atmel you will add to the this library),
"Samtec" (for all parts from Samtec you will add to the this library),
...
with Altium open and running, click on file tab (left bottom corner of work space, find "Blank Project (library Package)" and click on it. A new Library Project will be created.
in Projects tab (next to the Files tab you clicked before) right click on the new library project and  add to the project a new PCB library and a new Schematic library.
save this project and its two added files in the "Resistors sub-folder" with proper names (such as Resistor.LibPkg, Resistors.SchLib, Resistors.PcbLib"
now add all Resistors Schematic symbols (each with its P/N as Design Item ID), Then Footprint with name such as "0402-0.4mm", "1206-1.2mm", ... and add to each symbol the correct footprint.
right click on "Resistors.LibPkg" within the Projects Area (left column of your screen) and compile it as integrated library. Don't forget to address compile errors and warnings.
Do these steps for all other libraries. You are going to have several compiled libraries 
Now in your real design project, try to find "Libraries tab" and click on "Libraries..." button and install the integrated libraries (if you can't find this tab go to the View menu/Desktop Layout/Default.) 
This way you always have your libraries for all projects. Whenever you have a new component, simply open the relevant library project, add the component and its footprint, and recompile.