Eagle library export issue

On 19/11/2016 6:09 a.m., Erik Arckens wrote:

When a library is extracted from a .brd file with the file/run ulp/exp-lbrs.ulp command then all separate parts are stored in individual little libraries in the projects folder where also the .sch and .brd files are.

 

When in the libraries folder a new library is created for that project and all individual little libraries are copied into this single new library then there still is no live link with the .brd and .sch file. Example: if I change a component in this new single library (for example the pad size from long to round) and activate the "update" button on the library menu, nothing changes in the open .brd file.

If however I make the change in the little individual library and press "update" there, then the component changes in the .brd open file.

 

How can I change this so that the new library is connected "live" to the corresponding .brd file?

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/209767

 

Hi, from the newsgroup

There are a few traps for a novice using this ULP. The ULP is fine but

you need to use Eagle correctly to benefit from it.

If you run the ULP from the board the extracted libraries only contain

packages as that is all the board file contains so run it from the

schematic to get the full devices.

You can extract the device all to one new library or many libraries.

Lets say you extract to many libraries, that way the names remain the same.

There are considerations here as the ULP is not to build you a library

that you can manipulate straight away to make changes to the board. The

intention is to just get the libraries from sch/brd pair you acquired

from somewhere. This is important as it came from a foreign environment.

Lets say your board consists of a single resistor and the original

designer got the part out of the Eagle supplied library rcl.lbr.

When you use the ULP you will get a new library called rcl.lbr created

so now in your PC you have two libraries with the same name and

potentially the same device and package name exists in both libraries.

When 'you' set up Eagle you set the directories where your libraries

live. If the path to your new library is not satisfied by these

directory settings then the loaded sch/brd design cannot reach the

library. So maybe now you add a new path at the end of those already

there for libraries so you can reach the new one. Still no good because

Eagle looks through all the paths in order for the named library/part so

there is a high chance, for our example, that the rcl library and part

will be one from one of the directories listed earlier in the list.

If you make a change to the resistor in the new rcl library, eagle will

always find the other (earlier) rcl library containing the same part and

update the design with that. So you will likely see no change.

When you update the board you need to do it from the board.

If you use 'Update all' then the directory paths mentioned above will be

used. Using 'Update', you specify a specific library.

The update in the library editor only updates the other portions of the

library that may be affected by your library change. Like modifying a

symbol used by many devices. Libraries don't know which boards use their

parts. Schematic and boards only retain the library name and part name,

not where the library lives.

The above is brief and not the full story but you will get the drift.

HTH

Warren

Thank you very much Warren, your answer is as complete and understandable as I could have wished!

Erik

Thank you very much Warren, your answer is as complete and understandable as I could have wished!

Erik