Good description here: https://www.eevblog.com/forum/altium/component-library-management/msg604147/#msg604147
Hey that looks familiar
![Cool 8)](https://www.eevblog.com/forum/Smileys/default/cool.gif)
One specific revision to my workflow (or "our" workflow, since it's not just me anymore) since writing that: multiple tables for different part types was kind of a pain to manage, so everything is in one table now, and component types are a top-level category field. Trying to transcribe a lot of key parameters into a database table is a waste of time IMO, so headline specs go into the part description, and for anything else there's a link to the datasheet (using the Altium db schema, you can add links to a right-click menu from the database, so this is super convenient).
IMO you don't need to mess with databases unless you need to manage multiple people working on design projects (or you have some spare time on your hands and like databases
)
Hard disagree, the main benefit of a database is in the ease of symbol and footprint reuse across multiple parts, and general ease of data management. It's much easier to deal with design and manufacturing data across a whole library when all of that is in a single place, as opposed to spread across hundreds or thousands of individual library files.
The downside of a dblib in the context of this thread is that it's not straightforward to manage changes to library files in concert with changes to the database. We have all of our library files in a git repo (no need for an altium project, you can just have them all in a folder somewhere and use an external git tool to handle changes), but putting the backing database into the repo isn't workable. It might work for a single user with a local Access or Excel file, but even then, Altium's ODBC connection probably plays havoc with updating the file via git, plus it's a binary file, which is less amenable to git anyway. I'm not sure how to solve that. I played with exporting the database to CSV, so that you could at least see changes to the database in the git history, but it adds a manual step to each change and it's a pain to get the formatting to be properly human-readable as a diff. Some way of directly using a plaintext file as the backing database would be nice.
One of my goals for the new year is to move to a SQL database that directly synchronizes with our MRP, and at that point it may make sense to manage changes to the library files via that database rather than via git. Haven't gotten very far with that idea yet, though.
Thanks for this suggestion. It sounds the kind of thing I am looking for. I have a main PC with Altium on but on occasion I will use a laptop so I need a certain level of portability that I think the database system will not allow.
You can make that work with a dblib. I have for many years using an Access database. As long as you have a way of keeping that file in sync between the two machines (offline-capable network drive, dropbox, etc) it's not a problem. Doing that with multiple users is where it gets tricky. At that point a VPN back to a network drive (or database server) at the office is probably the right move for remote work. Although remember: you only need access to the database/library when adding or updating components to the design. Once a component is in the design, its footprint and symbol data is cached in the project files, and you can do all of the design, layout, etc without touching the libraries at all. I think the only other exception is if you're using database parameters in outjobs, you would need to be able to reach the database to generate those outputs -- but that's pretty niche, all of the component parameters (that are visible in the component properties) will be accessible to the outjob.
To use these libraries in a new project do you link them in each time? You never install a library, you just add the SCH and PCB files to the new project each time?
If the library files are in a library project (whether it's a dblib or intlib or whatever), you just need to have that library installed. No need to add specific schlib or pcblib files to the project, the system handles all of that via the main library project/file.