Extract a symbol from a project to a library

Wim Cranen wrote:

I cannot imagine that this question is not asked before.

 

Introduction:

I've tried to find the answer in this forum and with Google as well, but without succes.

Only library to library answers. But I have got no library, just a complete Eagle project.

 

Now the question.

While having a complet project (.sch and .brd file), I want to use parts of the project in my own library.

How can I extract a symbol, complete with package to a library?

 

Cu, Wim.

 

First, you don't really need to extract the symbols/packages/devices to

your own library, but it does sometimes make things easier in the long run.

1.  Create your own library using File | New | Library.  If you keep it

in the default eagle lbr folder, it makes it easier to find if you give

it a name near the beginning of the alphabet; 0lib_name works good for

this.  Otherwise, you can save the library in your own directory and add

the folder location to the eagle path using Options | Directories.

2.  OPEN your new library for editing.

3.  Open your project schematic and click on the Show Properties icon

(bold 'i').  Click on any symbol and it will show you the name of the

symbol (gate), the name of the Package, the name of the Device, and the

Library they all came from.

4.  Switch windows to the eagle Control Panel and scroll down the

libraries the the one used, and expand it and locate the Device listed

earlier.  Right-click on the device name and select Copy to Library.

This will place a copy of the Device, including all Packages and Symbol

to your own Library.

5.  Switch back to your Library Editor, and you will see the copied

Device.  You may want to rename any of the device/package/symbol names

and possibly delete (Remove) any unwanted Packages associated with the

Device.  It is usually good practice to name the Symbol to match the

Device, just for ease of use.

6.  Now, all you have to do is repeat steps 3-5 for all unique symbols

in your project.

7.  Warning, your original project will still reference the original

Library and device names.  If you need to update it, you can use Replace

using your new library devices on each symbol in the project.  If you do

not rename any of the devices, you can try Rename old_libr = new_libr

for each library originally used.

8.  As a final check, you can Export the Schematic PartsList to a file

and verify that all devices are now from your new library.

Good Luck.

~Marvin

Wim Cranen wrote:

I cannot imagine that this question is not asked before.

 

Introduction:

I've tried to find the answer in this forum and with Google as well,

but without succes.

Only library to library answers. But I have got no library, just a

complete Eagle project.

 

Now the question.

While having a complet project (.sch and .brd file), I want to use

parts of the project in my own library. How can I extract a symbol,

complete with package to a library?

 

Cu, Wim.

Assuming you have received a project from another person and it has used

their personal library creations that dont exist in your copy of Eagle.

Open your project and the run the ULP

exp-project-lbr.ulp

Make a new library to receive all the project devices and then use library

to library techniques to get the one or two you want into your personal

libraries.

HTH

Warren