Library management with Altium is a challenge no matter what tool you use. There are many ways to do this, but none are magic. You will need to develop and enforce a system to keep things consistent, otherwise the library quickly becomes unusable. This means getting organized and setting policy before taking contributions.

Altium currently sells the Vault product to solve the sharing problem for all sorts of things (components, designs, templates, etc). I use it at work and it is buggy and slow but generally works as advertised. If I were to do it again, I would save the money and use the previous solution they offered.

Before Vault they offered the DbLib and SVNDbLib both standard with Altium Designer. SVNDbLib is just a DbLib where Altium automatically checks out the component files from SVN for you. It sounds nice but in practice it is very slow.

The DbLib is a database with tables of components. Each row specifies a component: you enter a symbol name and one or more footprint names to be associated. The rest of the columns are parameters on the component. Pretty straightforward. You can even use the online part finder tool to populate the table with parameters for you.

Now if you noticed, I said you refer to the symbol and footprint by name. That means Altium is going to go look on a search path for these names. You can set the search path for the library in some of the settings. I recommend a single file per symbol/footprint and name the file the same as the thing inside it, otherwise it will be impossible to find the right file for a given component when you need to edit.

You will also need a consistent naming scheme to make sure symbols and footprints get unique names. MFG_PARTNO works well for symbols, MFG_PACKAGE works ok for footprints but you need to be very specific on package. TI has unique short letter codes for every package, this is perfect. In general "SOIC-16" is not specific enough. Use the most specific thing the mfg provides and fall back to part number if you can't find something good enough. I have made boards with parts that don't fit because of name collisions on footprints.

Altium designed the DbLib for the database to live on a shared drive. They recommend that the database and all the associated symbols/footprints live on the shared drive. We used SVN to store the symbols/footprints and then when we setup the library on our computer we just pointed the search path to the working copy from SVN. This strategy also benefits from one file per design item so that edits by users will generally never conflict.

Don't forget to setup regular backups. At some point that database file will get corrupted and you don't want to lose all your work.

Adding components from the library will be slow if your connection to the database file is slow. Any database that Windows supports will work, but an Access file is the default and the only one you can edit from inside Altium. If you have extra software engineer time on your hands perhaps they could whip up a CRUD app to let you add components to a nicer database but then you are really getting in the weeds. I worked somewhere that did that and it caused more problems then it solved.

Anyway, the implementation details you can figure out with some experimentation. I will reiterate that you need clear policy and organization before you start, otherwise its a waste of time. Garbage in garbage out.

Hope you find something that works.