Stats

  • Locked Locked
  • Replies 2
  • Subscribers 167
  • Views 17403
  • 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

Allegro footprint was not found

Celestine

I am new to Allegro PCB Editor. I used Ultra Librarian to download some part symbols and footprints for some of the components I need in my design but I am having problem transferring this footprints of this parts from my cadence PSpice design to the PCB Editor(after creating the netlist). I see the footprints were created but I am unable to manually place them in the PCB design. However I am able to place the footprints of the parts that I made locally. I am guessing it has to do with the file location of this downloaded parts. If anyone have solved this before I would appreciate a step by step instruction 

  • Dale Peterson

     Celestine,

    Here is a basic check list for you to use to debug your problem. Make sure your go over any errors or warnings that occurred during net list importing. There are clues that can help you in debugging too.

    1. No spaces or illegal characters used in symbol names or folders

    2. Symbol names too long. If this is the case go to your top menu- Setup/User preferences /drawing in this form set "allegro_long_names_size to something bigger. 255 is the most. and will always work.

    3. make sure the your footprint names in your schematic matches foot print names in your library.

    4. Make sure you have all the part's files (*.dra, *.psm and *.pad for the pads) in your library folder. If you are missing the psm, load up the part in the library editor and hit save. It will create that missing file.  

    5. Check your library parts for both the part and the pads under Setup/User preferences/paths/library. In this form check under psmpath and padpath. Make sure the part paths are in there.

    6. Make sure the pin counts and pin names are the same called out in the schematic symbol and on the your footprint package.

    I hope this helps you.

    Cheers

  • LouShay
    Hi Celestine,

    I'm betting on number #5 :)

    The netlisting process from Allegro looks for footprints in a predefined location(s). The location(s) is set in the User Preference Editor. The ‘default path’ if you will, is the design directory (I assume that's why you're able to place your local FP's). To find footprints in other locations (usually a footprint library) you need to set the psmpath and padpath values accordingly. Setup > User Preferences --- -Paths -Library, then re-run Import > Netlist

    Best regards, -lou
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.