Parts library tidy up and now links broken in existing schematics

Hello Steve,

If I understand, you move some device from the library 'VOM1271', into the library 'MyParts', that is correct ?

In that case, the best way is to use the 'replace' tool in your schematic (with the board open).

- select the replace tool, and select the device in your new library,

- click on the parts in your drawing, to replace them with this new version from this new library.

(As an aside, it seems that Eagle makes updating from one version to the next a real pain. The lbr, cam, scr, ulp etc folders are all recreated and one has to drag items created in the older version into the new folders.  Painful.)

For that point, Eagle always installs in a different directory for each version. That is the only way to avoid problems in production/industrial environment.

- What if there is some thing wrong with  the new version? you still have the old one.

- How do you manage the changes between 2 versions of the same library, if you simply replace the old ones by the new ones....

- ...

According to me, the best way to work is to not change, edit, add documents in the folders created during the installation of Eagle.

You create your own folder (lbr, cam ....) for your own library/scripts/cam etc... You locate these every where you want.

Then in the Eagle control panel, you select 'option->directories' and you add the paths of your own folders, so Eagle will include them.

Hello Steve,

If I understand, you move some device from the library 'VOM1271', into the library 'MyParts', that is correct ?

In that case, the best way is to use the 'replace' tool in your schematic (with the board open).

- select the replace tool, and select the device in your new library,

- click on the parts in your drawing, to replace them with this new version from this new library.

(As an aside, it seems that Eagle makes updating from one version to the next a real pain. The lbr, cam, scr, ulp etc folders are all recreated and one has to drag items created in the older version into the new folders.  Painful.)

For that point, Eagle always installs in a different directory for each version. That is the only way to avoid problems in production/industrial environment.

- What if there is some thing wrong with  the new version? you still have the old one.

- How do you manage the changes between 2 versions of the same library, if you simply replace the old ones by the new ones....

- ...

According to me, the best way to work is to not change, edit, add documents in the folders created during the installation of Eagle.

You create your own folder (lbr, cam ....) for your own library/scripts/cam etc... You locate these every where you want.

Then in the Eagle control panel, you select 'option->directories' and you add the paths of your own folders, so Eagle will include them.

Thanks Guillaume.  The is very helpful.  Yes, that was exactly the case.  I had a collection of failed attempts, stupid names etc and decided to start a fresh library. A few follow-up questions if I may:

1. How do I delete or rename a device or package in a library?

2. When you download additional libraries I assume you place these in your equivalent of your "My Parts" library. Can Eagle be directed to use both this folder and the standard libraries installed when a version is downloaded?

Regards

Steve

Hi Steve,

1-Deleting /Renaming

  - You open the library, and then open the Symbol, Package or Device you want to Delete or Rename.

  - In menu you select 'Library-> rename' or 'Library-> remove' .

Note #1: When you rename: by default, Eagle will propose the current name. When you Delete, Eagle propose en empty name, you have to type the exact name of the Symbol, Package or Device you want to delete. This avoid to delete accidentally. But if you are lazy (like me ), instead of typing the exact name (Boring ! ), if I want to delete, I first use the Rename function, I copy the name (Ctrl + C) and I cancel the renaming. Then I use the delete, and instead of typing the name , I just paste it (Ctrl +V) !!!

Note #2: You can not delete a package or a symbol that is use in a device (in the same library). Delete the device fisrt.

Note #3: If you rename a Device, In your schematic, you will have to replace the part (like i explained).

Note #4: When I want to create a device, that is quite similar to an other device (in the same library). For example, you need a new op-amplifier, same package, same pining, but different reference, performance, supply or etc... Some time you may want to duplicate the device.

- in the control panel you develop your library (so you can see all the components).

- you open the library, and in the library editor you open the DEVICE you want to duplicate.

- you rename it with the new name, AND you DO NOT SAVE the library.

- in the control panel, since you didn't save your library, you still have the old device name.

- On the old name, your proceed a right click + 'copy to library'

- now in your library you have the old component, and a copy with his new name. (and you can save ! )

2- In Eagle I defined the library path like this :

$HOME/eagle/Lib Perso:$EAGLEDIR/lbr

This mean that eagle will use the library in my own personal library folder (My preeeecious, golum golum) AND the library installed when you installed your EAGLE.

Eage will automatically replace the $EAGLEDIR with the path of Eagle installation directory.

In my own personal library folder, I made different folders (linear, regulator, passive, etc...) in which there is other sub folder (for linear: ADC, DAC, Amplifiersetc..).

Eagle will browse and use all the sub-folder. So every thing is accessible and ordered in my own way.

In my own personal library folder, I add a 'download' sub-folder, in which there is my downloaded additional library.

Usually, I never directly use a component from a downloaded library or a Eagle installed library. First because I add my own attributes, and I change some details. And also because these library have too many components that I don't use.

So when I use a component from Eagle or download, that I need to edit a little, I copy the component in my own library ( I open my library, and in the control panel, right click + 'copy to library  on the component I want to copy). For example I have my own Resistor library.

Since I rarely directly use Eagle library, I mark them 'unused' (green dot in the control panel). So when I add a component, only my library is listed ! (it easier to found a component !)

An when I had to use a component, from a Eagle/or download, i had it from the control panel (while the schematic is open, in the control panel I select the component, then i click on ADD.

Guillaume.

Perfect.  This has been extremely helpful.  I have followed your advice.  Thanks!

I'm glad I could help you.