OrCAD Layout Footprint to Allegro Package

In OrCAD Layout:

   Create catalog of Layout library to generate .MAX file.

       
In Allegro
 
   Convert .MAX file to Allegro .BRD file using File...Import...CAD Translators...OrCAD Layout...Translate
   
      ( Will not work if you are in "component" mode.  Do File...New...
        and start a new empty "Board" file;  eg: A )
        
   run File ... Open ... ( .BRD file just created )
   
      ( Do you want to save the changes you made to " A.brd ? "  Click " NO " )
      ( A Warning box appears.  Click " OK " )
 
   run Tools ... Derive Connectivity
   
      All check boxes checked
   
   run Tools ... Database Check
   
      All check boxes checked

      Check
      
      Close
   
   run Tools ... Padstack ... Modify Library Padstack
   
      Click " OK "
   
   Setup ... Cross Section
   
      Delete PLANE layer

         ( Click on PLANE layer, rt-click, select Remove )
      
      Delete INNER layer
      
      Delete excess Dielectric layers
      
      Apply ... OK
      
   Save the .BRD file
   
   run Tools ... Padstack ... Modify Library Padstack
      
      Click " OK "
   
   run Tools ... Database Check

      All check boxes checked

        Check
      
        Close

   run File ... Export ... Libraries
   
      ( this can take a while )
      
      Close
   
   run File ... Open ... 
      
      Browse to the Package just created to check it out
      
      Choose " Files of type: " Symbol Drawing ( *.dra )
      
      ( Allegro opens in " component " mode )
      
      ( To view holes, Setup ... Design Parameters ... Display
        check boxes: " Display plated holes " and " Display non-plated holes " )