Actions
Forum Thread Details
  • State Verified Answer
  • Replies 6 replies
  • Answers 2 answers
  • Subscribers 180 subscribers
  • Views 2626 views
  • Users 0 members are here
Related

Custom device doesn't update after package editing

Former Member

Hey there,

 

I'm quite new to Eagle, so please don't throw rocks if I'm asking something basic.

I've created a custom device and after turning it into a real PCB I realized I need to modify some pads. I looked up the specific package in my library and performed the necessary changes. The problem is now that I can't get Eagle to allow me to use my updated device.

 

I am attaching a few pics to illustrate the problem:

- SPDT_device_library.png shows the device in my library. I have intentionally edited the pads on the sides to be asymmetrical, so that it would be easy to spot whether the device is updated or not

- Control panel view.png - back to my control panel, when I look inside the library, the old package is being displayed to me

- Using the device.png - not surprisingly, if I use the device in a new project, I get the old package with symmetrical side pads.

 

I can't find an explanation for what is happening here. It looks like there exists no instance of the old package. Yet somehow the device from my library is pooling out from somewhere and using the old package.

 

Your help is greatly appreciated,

Mihaela

Attachments:
image
image
image
  • 0

    Hi,

     

    Just a couple of suggestions to get the really simple possibilities out of the way first before trying to work out what else might be going on:

     

    a) Are you sure you saved the changes in the package editor before using it in the design? Really obvious and probably not the issue but I had to ask!

     

    b) Are you sure you are editing the copy of the library you think you are editing? I had a similar issue a while back and I found that the version of the library I had open in my library editor was in a different folder because I had been in the middle of re-structuring my libraries and my library path in EAGLE was pointing to a different copy! Needless to say I got right back to finishing off my re-structuring so that wouldn't happen again!

     

    Best Regards,

     

    Rachael

  • 0

    Try exporting the source (.scr).  Take a look at the source with a simple editor.  Look for the device-in-question's package.  That may give you a hint.

     

    GP

  • 0

    Hi

     

    If you have made the change in the library and saved it.

    Then in the board you performed a library update or update all

    and the problem persists.

    Or if you ADD the part and it is the unmodified one, then I strongly

    suspect the following:

     

    You are accessing a similarly named library in your environment.

    You could confirm another library of the same name exists by searching for

    eeg_parts.lbr

     

    There is a few reason you can target the other file.

    In Control Panel > Options > Directories > Libraries

    if there are multiple paths to library folders, they are checked left to

    right so if you library name is found in another folder, and the device

    name matches, that's the one that gets used.

     

    Another way, if you use projects, comes from your eagle.epf file in the

    project folder. There is one of these files for each project. In it there

    are paths to used library files and hence if a project came from different

    instance of Eagle it could point to the other library location. You can

    un-use all libraries by entering into the command line

    USE -*

    That will un-use all the libraries. Then you should 'use' the ones you want

    again.

     

    HTH

    Warren

     

     

     

     

    --

    Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

     

  • 0 in reply to rachaelp

    Hi Rachael,

     

    Thank you for pointing out the obvious possible sources. Many times the unexpected behaviour comes from unnoticed small mistakes like the ones you mentioned. I had checked the two options you identified, but I think it's very good practice to start with them.

     

    Best,

    Mihaela

  • 0 in reply to glennp17321

    Hi GP,

     

    Your tip led me to exporting the part list (I didn't know where to export the scr from) and noticing a silly mistake I had made. I had changed the library name as the initial one was a bit confusing (in the Control Panel -> I selected the library and hit Rename). And then I changed the package I was interested in.

    In the exported partlist I noticed that the parts that wouldn't update were still considered to belong to a library having the old name. I was assuming that when the library name got changed, the included parts from my project would also update their library source name, but that is not the case. I have now changed the library name back to its original value and the parts from my project updated properly.

     

    Thank you for your patience with noob question,

    Mihaela

  • 0 in reply to Former Member

    Hi Mihaela,

     

    Rather than renaming your library back to allow the update, you could instead have right clicked on the component in question in the schematics and selected 'Replace' from the context menu and then picked the part from your renamed library.

     

    Anyway, I am glad to hear you got to the bottom of your issue and you now have your design updated, I just wanted to let you know of this alternative for the future.

     

    Best Regards,


    Rachael