Before you follow the procedure that follows, you must either already have the library files in .MAX format or have a working version of OrCAD Layout to create the library files. OrCAD Layout was last shipped from Cadence in version 16.2 and is no longer available from the Cadence support download site.


This solution describes the footprint library translation for those migrating to Cadence® Allegro® technology PCB Editor from OrCAD Layout.   


OrCAD Layout Footprint Libraries

  1. Open OrCAD Layout. In the Session Frame select Tools > Catalog > Create.


  2. Select a footprint library and create a .MAX file using the Catalog Tool.


  3. Select the OK button to create the .MAX file.

  4. Select Open from the File drop-menu of the Session Frame and navigate to the location of the library .MAX file.
    An example of a library .MAX file opened for viewing in OrCAD Layout is shown in the screen image below.


  5. Save and close the Layout .MAX file.


Allegro Technology PCB Editor

  1. Open the Allegro technology PCB Editor and create a blank or "empty" board file (.brd).

  2. Select Import > OrCAD Layout from the File drop-menu.


    Notes: There are two required or mandatory requirements that ensure the Allegro technology PCB Editor footprint footprint is a real footprint. There needs to be at least one pin and a reference designator on the layer Class Ref Des Subclass Assembly_Top.

    Unlike Layout certain characters may not be used in the Allegro technology PCB editor environment. Certain characters such as ".", "/", and spaces are stripped out during the translation process.

  3. In the OrCAD Layout to Allegro dialog box, select the Layout Library .MAX file you want to translate to PCB Editor/Allegro The translated board file will be in the same directory as the .MAX file.


  4. Click Translate.

  5. When the translation is complete, the "log" file for the translation will appear to inform you if there were any errors during the translation process. Close the resulting .log file.


  6. You should now see all the translated footprint patters from the OrCAD Layout library present in the Open <translation>.brd file.

  7. The .log file opens to show how many items are translated.

  8. Close the Translation dialog box and the .log file windows when you are finished.

  9. Select the File > Export > Libraries menu items to extract PCB Editor/Allegro symbols from this .brd file.


  10. The Export Libraries dialog window appears. Make sure to select all Elements and the directory you want to place the symbols It is recommended that you use the same directory where the <translation>.brd file is located until you examine and verify the resulting symbols and padstacks.


  11. Move the Translated Padstacks and Symbols to your standard user library directory.