Making new libraries in Cadstar?

[grizedale]

Hello,


My cadstar libraries were started by other people......i have added to them and they have become messy.

I want to start again with completely fresh, empty libraries.

In windows i created a file, and then in TOOLS>OPTIONS>LIBRARY PATHS, i added this file to my libraries...but when i press "OK" it warns me that certain files for the library path do not exist.

...it names these files as pcb.lib, symbol.lib, docsym.lib , parts.lib.

..it asks me if i wish to disable these library types for the path.

I am not sure what to do about this warning.

Do you know about this warning, and how i can start with new, fresh libraries in CADSTAR?

 

[marce]

Just create new libraries in the location specified, dont disable the library types. The library disable feature is a tick box in the window you specified. This is usefull if you have multipe parts libraries from different sources kept in different locations for data management but want one footprint library, etc.

 

[Mattylad]

Do not create a file in Windows Explorer ??

To start with completely fresh libraries:

Use Windows Explorer to make yourself a new library folder, perhaps as Cadstar 12.1\Library after renaming the existing folder to "oldlibrary" etc.

In the Library Editor (or the Design Editor).

Copy this path and use it to create a new library path in Tools\Options\Library paths tab. (or browse to it)
Once the path is setup, ignore the warning about disabling the files, this will be because the files do not exist yet so say no.

Create the binary files:
a) Then in Libraries\Schematic Symbols use "Create" to make a new symbol library, I suggest you use SCM in the name somewhere to distinguish that it is a Schematic symbol library.

b) in Libraries\PCB Components use "Create" to make a new component library, I suggest you use PCB in the name somewhere to distinguish that it is a PCB component library.

c) in Libraries\Documentation Symbols use "Create" to make a new Documentation symbol library, I suggest you use Docsym in the name somewhere to distinguish that it is a Documentation symbol library.

You may wish to find a known good symbol/component in the old libraries, open them then change to the new library and save them to start these off.

In the Tools\Options\Library paths tab you may note that the PCB and Schematic/Docsym library files point to the ones you just created.

Then in the Library Editor.
Create the part file(s):

Use File\New\Part Library.
Add your first part here. (this can be copied from an existing library to start you off), preferably using the symbol and component used above

You may wish to create library files for each type of component I.E. Resistors, Diodes, Relays, Hardware, Micro, BGA etc.
You may also wish to differentiate between SMT and PTH with different part library files. I.E. PTH Resistors.lib, SMT Resistors.lib.

More library files maybe, but it allows you to seperate parts better and search better based on the type of part when using the slide out library window.

Creating the parts indexing:
In either Design Editor or the Library Editor.
Using Libraries\Parts, Select the "Libraries" button and add your new part library files here, removing the basic "parts" one listed.

When you exit this screen it will prompt you to reindex the libraries, say yes and read the report.
If there are any errors in the parts library it will be for the library listed above the error line, hopefully there will not be.

Regarding the above comment about copying the old symbol/component into your new library etc.

Before doing ANY of the above, sit down and plan your new library, plan how it will be used, what layers you need and their names & use, what line codes, text codes etc you need. Create a document that details ALL aspects of your new library, what linecode you will use for symbol outlines, component placement/Silkscreen and assembly outlines, 3D 1:1 outlines, pad naming conventions, reassignment use, attributes needed etc, etc, etc.

Consider EVERYTHING. (including the effect on existing design files) Oh and go Metric.

Document it, discuss it with others that may use it (including design,assembly, PnP, test and the janitor), approve it, procedure it, issue it, follow it, then reassess it etc.

Only when you have followed the line above make the files, otherwise you may be wasting your time if your in a company/business.

Good luck.
Starting a completely new library is a big jump for a company as it involves a lot of work but allows you to reap the benefits.
You also have to consider remaking your default files, your colour files, et all.

Any problems - we are here to help (and have you got a maintenance contract - they can help too :wink: ).

 

[marce]

Nowthen Matt :lol:
On a more serious note, keep things simple when doing a new library. I think it is the best way of both getting to know a system inside out and having full control over your data.

https://www.frontdoor.biz/HowToPCB/HowToPCB-extra/CADlib.pdf

Below are a couple of examples of my SCM default line and text codes, I use generic names for symbol outlines etc and text so that they are easy to choose when creating a symbol and make for consistent design from one symbol to the next. I do the same for components and documentation. I have used this format for many years and many libraries, and with the codes having a genetic name I can alter sizes to cater for different requirements, whereas where you use a specific size in a name things get messy, such as the standard text codes that come with Cadstar.