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

  • Quote:

    But the library I got the part from is an Eagle-supplied library,

     

     

    There's the real problem.  Some mistakes can't be fixed after the fact.

    This is one of them.

     

    Next time think of this before painting yourself into a corner.  The advice

    not to use the Eagle libraries directly is given here often, and should be

    obvious from a little thought anyway.

     

    That all said, changing one part is not likely to rip up a lot of the

    routing.  If I remeber right, the ripup will only go as far as the next

    part or net junction.

    --

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

     

  • in reply to autodeskguest

    On 07/29/2014 02:30 PM, Olin Lathrop wrote:

    Quote:

    But the library I got the part from is an Eagle-supplied library,

     

    There's the real problem.  Some mistakes can't be fixed after the fact.

    This is one of them.

     

    Next time think of this before painting yourself into a corner.

     

    Robert,

     

    It's not as bad as Olin infers.  There's a way to do this without

    disturbing your layout.

     

    Try this:

    I couldn't find where Eagle keeps the path to the library stored in the

    schematic, but it does keep the name of the library.  Thus, this stands

    a good chance of working.  You could copy the eagle library in question

    to your own personal lbr directory WITHOUT changing the name.  Make sure

    your personal directory occurs before the eagle directory in the library

    directory path.  Drop the eagle library from use, and use yours

    instead.  Then modify the symbol, save it, and do a library update.

    I've done this with the RCL library (and others) with success across

    updates and upgrades.

     

    If that doesn't work, try this:

    Open your personal library and copy the DEVICE from the eagle library to

    yours.  Modify the symbol as needed and save it.  Add this personal

    library to your USE list.  Then replace the device on your schematic

    with the device in your personal library.

     

    Neither one of these methods should change the board layout, provided of

    course, that the package is identical.  No rip-up and reroute should be

    required.  That said, do a ratsnest to check for air wires and drc just

    to be sure.

     

    HTH,

        - Chuck

     

     

  • in reply to dukepro

    EAGLE stores everything in the board and schematic files.  I'd suggest

    using the exp-lbrs.ulp to extract the libraries back out from your design

    into a local directory, then make your changes and use the "update" command

    to pull them back in...

    --

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

     

Reply
  • in reply to dukepro

    EAGLE stores everything in the board and schematic files.  I'd suggest

    using the exp-lbrs.ulp to extract the libraries back out from your design

    into a local directory, then make your changes and use the "update" command

    to pull them back in...

    --

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

     

Children
No Data