• Skip to main content
  • Skip to search
  • Skip to footer
Cadence Home
  • This search text may be transcribed, used, stored, or accessed by our third-party service providers per our Cookie Policy and Privacy Policy.

  1. Community Forums
  2. Allegro X PCB Editor
  3. Change Connect Pin to Mechanical

Stats

  • Replies 11
  • Subscribers 160
  • Views 22356
  • Members are here 0
More Content

Change Connect Pin to Mechanical

archive
archive over 17 years ago

Other than deleting a Connect pin and inserting a Mechanical pin in it's place, is there a method of changing a Connect pin to Mechanical ?


Originally posted in cdnusers.org by dschaefer
  • Sign in to reply
  • Cancel
  • archive
    archive over 17 years ago

    Just change your find filter so Text is checked, delete the pin number text and you are good to go. Of course this can only be done inside of the Allegro symbol (.dra) and not the layout (.brd).

    Hope this helps,
    Mike Catrambone
    UTStarcom, Inc.


    Originally posted in cdnusers.org by mcatramb91
    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Cancel
  • archive
    archive over 17 years ago

    Hey there,
    What about the other way around? Changing a mechanical pin to a connect pin?

    Jackie


    Originally posted in cdnusers.org by Jackie
    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Cancel
  • archive
    archive over 17 years ago

    It's better to replace the mechanical pin to a connect pin inside symble (.dra) using "Add pin" option.


    Originally posted in cdnusers.org by shiva
    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Cancel
  • archive
    archive over 17 years ago

    Jackie,

    There is a way to convert a mechanical pin to a connect pin but it should only be used when you have multiple(many) pins to convert and it would take too long to replace them manually using "Add Pin".

    All you need to do is to create a sub-drawing (File > Export > Sub-Drawing) of just the pins using x 0 0 as your origin point then manually update the sub-drawing file (.clp) file by globally replacing the following string: (add 99 as your pin number)

    -->From
    _clpInitPinText(_clp_pin_text "" 0:0)

    -->To
    _clpInitPinText(_clp_pin_text "99" 0:0)

    Once you make these change you can deleted the existing mechanical pins and import the modified sub-drawing (File > Import > Sub-Drawing) into your symbol using x 0 0 as your insertion point. Now the pins will have an pin number associated to them which makes them a connect pin and using Edit > Text you can change the pin number place holder 99 to the correct pin number.
    Doing it this way you don't have to stress on placing the new connect pins at the exact same location as the existing mechanical pins and all you need to do is update the attached pin numbers.

    Like I said before if you only have a couple mechanical pins to convert to connect pins then it would be fast to just replace them using "Add Pin" as Shiva indicated but if you have lots of mechanical pins to convert it is just faster going the sub-drawing Export/Import route.

    Hope this helps,
    Mike Catrambone
    UTStarcom, Inc.


    Originally posted in cdnusers.org by mcatramb91
    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Cancel
  • archive
    archive over 17 years ago

    Mike,

    Thanks for the replies. Would have hoped that there would be better support within Allegro for converting between Mechanical and Connect pins. I guess not something most do too often if libraries were created from scratch in Allegro, but for those of us transitioning and converting libraries from other tools such as OrCad Layout it would really help.


    Originally posted in cdnusers.org by dschaefer
    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Cancel
>
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.

© 2025 Cadence Design Systems, Inc. All Rights Reserved.

  • Terms of Use
  • Privacy
  • Cookie Policy
  • US Trademarks
  • Do Not Sell or Share My Personal Information