Component search building own database at what value?

[Houseman]

Moving from Eagle to Altium has shown me the "apparent" value to think a schematic as starting from building your own precise component list via a part search and then draw a fitted schematic...
This solves future problems like BOM and other issues.
Eagle for my personal low experience was all about throwing on the sheet a bunch of symbols for passive components not really related to the precise part used in manufacturing ( 0805 10k resistor) and then search during PCB drawing the details.

So why for each project build your own SCH library full of components starting from empty symbol and footprint rather than searching from the supplier the ready model and footprint?

Is there a way in Manufacturer part search to add the ready component to your personal library instead of copying and pasting the symbols, the footprints and so on wasting a lot of hours?
Best regards and thanks

[thm_w]

You can use Altium like eagle if you want, as I do, put in generic passive components.

Why are you building a schematic library just for one project though?
If necessary when you are finished you can create the library: https://resources.altium.com/p/quickly-create-project-libraries-from-the-schematic

[ajb]

There are a number ways to deal with libraries in Altium, and there's not really a right answer.  If you're actually making a new library from scratch for every project, though, I don't think that's a good use of your time.  Component data including footprints and sch symbols are stored in the projects where they're used, so you never have to worry about losing that information if the project files are separated from your local libraries. 

Using the manufacturer part search and the ready-made symbols and footprints you find there can be a fast solution, but then you are relying on those things 1) being correct and 2) having the data and formatting that you want.  I would hope that those symbols and footprints would be pretty decent, but it's always a good idea to verify for yourself that everything is correct before using them.  If you're working on your own then it's up to you how much to care about how consistent the symbols and footprints are and what level of information you want in them, but if you're working as part of a team then that matters a lot more.  Big companies may have dedicated people (or a whole department) to serve as librarians, making sure all of the symbols and footprints are correct and comply with company standards. 

Consistency and correctness are especially important with footprint design, because the quality of the footprint directly determines the quality of the fabrication and documentation outputs.  The quality of fabrication outputs directly affect the quality and reliability of the finished product--getting the right amount of solder paste onto the board and in the right shape, for example, is critical to preventing bridging and tombstoning. 

Consistency is less critical on schematic symbols, and it's easy for engineering types to dismiss the graphic qualities of schematic symbols as irrelevant aesthetic nonsense, but the reality is that creating a good schematic is as much a matter of graphic design as it is engineering.  A good schematic is clear, well organized, and easy to read, and makes the most important things most prominent.  Having good symbols is an essential part of that.  Personally I just plain hate the default graphic style and colors in most Altium sch symbols, so I always create my own.  That way I can ensure that fonts and styles are consistent, the relative sizes of components makes sense, etc, which all makes for a better schematic.

However you acquire or create your symbols and footprints, I strongly recommend looking into creating a DbLib for your library.  These use a database (which can be an Excel file, an Access database, or a full SQL server or whatever) to link schematic symbols, PCB footprints, and whatever other data you want into a single library.  It makes it incredibly easy to reuse sch symbols and footprints and add new components--if I want to add a new resistor value, I can just duplicate one row for a similar part in the database, edit the value, manufacturer part number, whatever, then hit F5 in Altium's component panel and place it in the schematic.  There are a number of threads here on how to organize DbLibs if you just do a search.

[thomasgreenezru]

is eagle better than Altium tho? In general, where can I read more about databases and stuff? I would appreciate any help. The only useful thing that I have found so far is the flashcard from https://quizzes.studymoose.com/flashcards/databases/ about databases. Found some really interesting information on that website, but I feel like I need to find more. If you can help, I'd be really happy.

[ajawamnet]

The way of done parts for years:

https://www.ajawamnet.com/ajawamnet/parts/parts.htm

I have so many clients that have so many different requirements as to lifecycle management - and most do NOT own Altium.   This way, they have control over what Form Fit Function choices are, regardless if I'm around or not.   Also - most of my clients have other stuff that they need to track - mechanicals, enclosures, ancillary gear - that using the Altium wiz bang thing ain't so good.

Another thing is a lot of my clients are ITAR or something like AS9100 - so I can't just go willy nilly search for stuff.  So that's another limitation to the whole ActiveBOM/Altium on line thing.  A lot of my clients use ORCAD and they too are forbidden from using stuff like CIS/CIP.