Tips for creating a Library

[khanna_gunjan]

Hello All,

I am in a process of creating library database for our company and would like your help to provide me with certain tips to begin with.

Do's and Don'ts etc.

Thanks for your time.

 

[Mattylad]

1) Do let people know what software you are asking about.

2) Do write down how your library will be established, what the structure will be, what settings for certain items will be (like silkscreen line width) etc.

3) Do ensure that everyone keeps to #2

4) Do not just make loads of parts - they may not be needed, libraries are usually created on a "need this part" basis.

5) Do discuss the library with every department that gets involved with a PCB, from buying, assembly, test, repairs, service etc so that you can be completely sure what features you need to add to your library items.

6) Check everything - include a checking procedure. Not doing so can lead to mistakes being included in a real PCB.

How about you let us know your ideas for your library first, that way we can tell you if your making a mistake or not.


P.S. this can take a long time and a lot of effort - however the time & effort is usually worth it if you do it correctly and include everything that you may need during board design & use.

 

[TraceRouter]

What Mattylad said is excellent advice!! The biggest thing is to take your time and do it right, a bad library will make it difficult to create good designs effectively. You also might want to look at Tom Hausherr's Blog (**broken link removed**) since he just finished a 6 part series on libraries.

 

[Mattylad]

Cheers for the link TR, I never knew Tom had a new blog - I'll link his to mine. Tom duz good stuff!

 

[TraceRouter]

What is the address to your blog?

 

[khanna_gunjan]

How about you let us know your ideas for your library first, that way we can tell you if your making a mistake or not. .

My plan is to :
1. at first define the component grouping.
2. proceeding with the min. information to be linked with each part ex. part number, manufacturer, footprint etc etc.
3. defining the design rules for both symbol and footprint generation.
4. creating a Checklist for the created parts.

something else that might be missing?

regards

 

[TraceRouter]

Looks like Tom has added 2 new library blog entries since I posted this suggestion. His blog is located at **broken link removed**

 

[altf4]

Don't forget to properly label and describe the devices in the library. I like to list out some distributer sku numbers so when its time to assemble the BOM I can find the parts easy.

 

[Mattylad]

In CADSTAR libraries we add attributes, one per different bit of information that we want to store.
These will be for all sorts of things including Manufacturers name, part number, suppliers name and stock code, rosh compliance, value, tolerance, who created the part, who approved it and so on.

The information allows bespoke reports to be made that can output any of these bits of information based on the BOM.


Before you actually start filling out your library sit down and discuss everything that is going into the library structure, discuss it with everyone that is involved ihn the manufacturing process from buying,board manufacture, assembly, test, sales (not forgetting IT dept) etc.

Then at least you are able to make informed decisions on what to put in it and how the information may be used and how to use it.

Decide on what standard you want to follow for footprints (I.E. IPC7351) what outlines and line widths you want, what fonts and font sizes to use etc and write them all down.

Use them, test them and then make them a standard - use them on ALL your symbols and footprints.

Make your footprints all using metric pad codes, mm drill sizes.
If you can name the pad codes, line widths, text codes etc then name them appropriate they are being used on.

I name my pad codes appropriate to how they are used.

I.E. not pad code 1, pad code 2 etc but more.
SM Rectangle 1.0mmx1.2mm
PTH Circle 1.5mmx0.8mm drill.
NPTH Circle 3.5mm

 

[gigahertz]

Hello all,

This is a very good topic and very important. I'm also looking to setup a nice library. I mainly use pads and altium and thinking of making some sort of database that can be used for both. I also got the mentor graphics wizard to make libraries for both these programs.

Does anyone have experience doing something like this with a database? thanks

 

[marce]

As Tom Hausherr has been mentioned twice, I would suggest very strongly that you use the IPC-7351 standard for your footprints instead of trying to do your own. Look for Toms 'Cad libray of the future'. There is a lot of documentation relating to the standard and most (all) footprints you'll ever need have been created. If you want to go one step further look at the IPC 2611, 2612 series, with info for schematic sysmbols and documentation. There are numerous IPC standards and information for PCB design, and when you have boards made ALL manufacturers will use IPC standards to fabricate and qualify your designs, so its worth using IPC standards.
I've done two IPC format libraries, one for Allegro and one for Cadstar, the latter using the wizard. I just created all the footprints in one go, but only load them into the library when required. The IPC-7351 format I use is without the height, so only have one generic RESC1608 footprint, (resistor chip 1608) instead of several with different component hights. When transferring to the 3D system via IDF all models are created with the packages maximum height to avoid problems.

 

[gigahertz]

Thank you marce for your reply and valuable feedback. I have one basic question you might be able to help with: if I just use the maximum height I find, for a given set of components of caps and resistors, this won't cause any potential assembly problems if I use a component that has a thinner height? This would really simplify things to be able to have one generic footprint for at least the caps and resistors, otherwise it seems it will be a headache making 10s or 100s of footprints for a particular size like 0402 etc.

 

[marce]

For checking spacing using the max height per footprint means for a given assembly ALL lower height components will fit. For 99% of all designs this should suffice. The origional wizzard etc I used allowed for either libraries with multiple footprints with Height as part of the package name or single footprint without Height as part of the name.
Having looked at the most recent release of the spec, height in the name dosn't seem an option any more, yet the wizzard allowed it! In my view for some components I dont think it is required, I shall forward my views to the IPC-7351 committee and see what they think.
**broken link removed**