Stats

  • Locked Locked
  • Replies 8
  • Subscribers 168
  • Views 18690
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Updating library symbols from PCB editor?

JFord

Hi,

 

(Using version 16.2)  I'm new to Allegro so please forgive me if this question has been asked before.  I have a part that is placed and routed on a pcb.  Some of the pin locations on the part had to be modified at the board level to accommodate routing, and now the library part is out of date with respect to the pcb.  Is there a way to update the library part with the part on the pcb?

  • hpattie

    In your board file, under the File tab, you can export libraries. This will bring up the Export Libraries menu.

    Select the part types you wish to export, and a location to store them.

    You can then copy the symbol you have modified back to the originating library from the export directory.

    Regards,

    Harold Pattie

    harold.pattie@ericsson.com

     

  • JFord

     I tried this, and the symbol in the newly created library is the same as the old library symbol (it was not updated to reflect the latest changes that were made at the board level)

     

    Maybe I missed something?

     

    Thanks,

     

    Jason

  • redwire

     Run the report "Symbol Library Path" and see where your *real* symbol is located. I bet you find Allegro is finding the first (yet wrong) symbol.  Putting the compiled .psm file in the correct path will correct the issue.

    If that is not it...check your logfiles after the update.  Are there missing padstacks? :)

  • oldmouldy

    Did you run Place>Update Symbols and select the symbol that you want to update?

    Copies of the library parts are stored in the board database, not picked up from the symbol library path, the Update Symbols process gets any changes reflected in the board database copies.

  • Rik Lee

    When you export libraries from the board design it will export the symbol definition - as it is in the library. If you have modified pin locations and want to export those you will need to use Allegro's subdrawing capability.

    I prefer to use 0, 0 as a location when I am using Allegro's subdrawing capabilities as I can easily type that location into drawing to ensure I have the correct relationships amongst elements.

    Give this a try.

    o File >Export >Subdrawing; With 'pins' on in the Find Filter window select the symbol. This will select the pins. Select an xy location by either digitizing a point or typing a location at the Allegro command line. Save the subdrawing.

    o Open the library symbol.
    o Delete all pins.
    o File>Import >Subdrawing. Select the subdrawing which contains the pins and add the pins at the required location.
    o Save the drawing.

    ~Rik

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.