Stats

  • Replies 4
  • Subscribers 69
  • Views 1523
  • Members are here 0
More Content

How to copy a cline or routed trace created in APD+ into Allegro PCB Editor

SaiPavanl

I recently faced an issue while working with routed traces in APD+ and Allegro PCB Editor. Specifically, I wanted to copy a routed trace from an APD+ mcm file to an Allegro PCB Editor brd file. However, it seemed that clipping of routed traces was not supported between the two tools.

After some digging, I found a workaround that I'd like to share with the community.

Routed traces or clines are represented differently in APD+ and Allegro PCB Editor. In APD+, they are represented as CONDUCTOR elements, while in Allegro PCB Editor, they are represented as ETCH elements.

Here are the steps to achieve this:

1. Open a mcm file in APD+ and check the representation of cline by using Display > Element.

2. Go to File > Export > Sub-Drawing and export this cline from the database. Notice that it is represented as CONDUCTOR in the subdrawing clp file.

3.Replace and change the CONDUCTOR in the clp file to ETCH as follows

4.Open the brd file in Allegro PCB Editor and go to File > Import > Sub-Drawing to import this clp file. This will import the routed trace or cline from the APD+ database to the Allegro PCB Editor database.

Note: Make sure you have the same netlist information in both databases to ensure correct connectivity.

You can also use this procedure to import a cline from Allegro PCB Editor to APD+. Simply replace the ETCH element with the CONDUCTOR element in the clip file before importing it into the APD+ database.

I hope this solution helps others who may be facing a similar issue.

  • masamasa

    hello

     

    this is useful information.

     

    what is the definition of conductor and etch, anyway?

     

    regards

    masa

  • SaiPavanl
    in reply to masamasa

    Hello masa, this is due to difference in fabrication process for IC Package and PCB. In PCB for laying out traces Subtractive etching (i,e Pattern plating or etch-back) is used and for IC Packaging Semi Additive process is used for fine features.

  • MO202507021411

    Thank for sharing such a helpful information. I have learned a lot.

  • DavidJHutchins
    in reply to MO202507021411

    Cadence provides the routine named 'axlMapClassName' which returns the appropriate class name based on the type of product,

    below are examples from the documentation:

      EXAMPLES
             1) in APD
                 axlMapClassName("ETCH") -> "CONDUCTOR"
             2) while in Allegro
                 axlMapClassName("ETCH") -> "ETCH"

    Another issue is the first & last 'etch' layer names used to be different:

        in Allegro they are "TOP" & "BOTTOM"

        in APD they are "SURFACE" & "BASE"

    That may have changed since I no longer use APD...

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.