Actions
Forum Thread Details
  • Replies 7 replies
  • Subscribers 179 subscribers
  • Views 3534 views
  • Users 0 members are here
Related

How to change libraries after routing

autodeskguest

I have a design that is completely routed (by hand).  Now I want to

change the look of a symbol used in the schematic.  But I don't want

to disturb any of the existing routing, so I can't delete the part and

add in a revised version of it.  I could edit the library and update.

That would do it.  But the library I got the part from is an

Eagle-supplied library, and I don't want to get into the maintenance

headache of tracking changes to Eagle libraries.  I would much rather

make a duplicate of the part in a custom library of my own, and then

have the part reference my custom library for updating instead of the

Eagle library.  But I don't know how to do that without disturbing the

routing to the part on the PCB.  It is only the schematic that should

be affected.  Is there any way out of this short of editing the Eagle

library this part came from?  I am considering editing the raw XML of

the schematic, finding the library reference, and changing it, but is

that safe?  I mean, what if my library version was accidentally

different in the package too?  What would Eagle do when updating from

a library where the package is inconsistent with the connections in

the PCB?

 

 

 

Robert Scott

Hopkins, MN

 

Parents

  • Hi,

    It's possible to change your symbol without risk and it's quite easy.

    • Start to create a new library, (or open one of your own library). Usually I name it in a way that It could not be mistaken with Eagle's ones, and I store it in an other directory.
    • Then, while your library is open, search in the control panel the device you want to modify. Use a right-click on this device, and select copy to library. This will copy the component into your library (symbol+device+package(s)).
    • You can edit your device and change the symbol, rename it etc...
    • You save your library.
    • You open your schematic (and board) if they don't, and you use the replace tool, to replace the device (from original library) with the device of your new library.
    • In that way you keep the eagle's librarys clean, and you limit the risk, since you just edit an 'already good' device.

     

    Be careful:

    If you have changed the symbol, but not the names of the pins of the symbol, Eagle will adapt the new symbol, and there will be no change in you board. In the schematic you may re-arrange your wire, because it could look messy (but there will no mix-up in the net list) .

    If you changed the pin names of your symbol, Eagle will try to retrieve the pin by their location. So If you want to change the pin names and their position, the best way would be to it in 2 separate steps, first just renames pin, replace your device with the new version. Then edit again you new library, change the symbol, but not the pin names. Then in you project, proceed a library update.

    If Eagle can not replace with the new symbol without risk of mix-up, Eagle will display a warning or error.

    Good luck.

Reply

  • Hi,

    It's possible to change your symbol without risk and it's quite easy.

    • Start to create a new library, (or open one of your own library). Usually I name it in a way that It could not be mistaken with Eagle's ones, and I store it in an other directory.
    • Then, while your library is open, search in the control panel the device you want to modify. Use a right-click on this device, and select copy to library. This will copy the component into your library (symbol+device+package(s)).
    • You can edit your device and change the symbol, rename it etc...
    • You save your library.
    • You open your schematic (and board) if they don't, and you use the replace tool, to replace the device (from original library) with the device of your new library.
    • In that way you keep the eagle's librarys clean, and you limit the risk, since you just edit an 'already good' device.

     

    Be careful:

    If you have changed the symbol, but not the names of the pins of the symbol, Eagle will adapt the new symbol, and there will be no change in you board. In the schematic you may re-arrange your wire, because it could look messy (but there will no mix-up in the net list) .

    If you changed the pin names of your symbol, Eagle will try to retrieve the pin by their location. So If you want to change the pin names and their position, the best way would be to it in 2 separate steps, first just renames pin, replace your device with the new version. Then edit again you new library, change the symbol, but not the pin names. Then in you project, proceed a library update.

    If Eagle can not replace with the new symbol without risk of mix-up, Eagle will display a warning or error.

    Good luck.

Children