The OrCAD Layout translator enables you to import OrCAD Layout max files into Allegro PCB Editor (versions 17.2 and 17.4). However, the Layout translator is built on a 32 bit platform while Allegro PCB Editor 17.2/17.4 is built on a 64 bit platform. Consequently, this feature is not a supported feature. Beginning with QIR3 (Hotfix s016) and application versions 17.2 and greater, you may enable this feature using an "unsupported variable" as described in the steps that follow.  


  1. Open Allegro PCB Editor and select the menu items: Setup > User Preferences.


  2. Select Unsupported from the Categories list. Notice how the selection controls in the dialog update.
  3. Select the layout2allegro_unsupported check box.
  4. Review the summary description.
  5. Click the OK button to apply and save the updated selection.
  6. Restart Allegro PCB Editor.
  7. Select the menu items File > Import > CAD Translators to import OrCAD Layout max files into Allegro PCB Editor.

Troubleshooting Potential Issues

The following notes may help you if you run into an issue during the translation process.

Before translating your Layout design to Allegro PCB Editor:

  • Avoid using characters such as $, ~, @, #, %, ^, &, *, ( , ), -, =, ', \, ", [, ], ?, /, <, >, !, . , ; , { , } , +, |  in reference designator and symbol names in Layout. Otherwise, the translator cannot convert the reference designator and symbol names correctly.
  • Clean up the design in Layout by using the Auto - Cleanup Design menu command or by exporting the design to a .min format and then importing it to a .max format.
  • Enable all layers on which routing has occurred in Layout.
  • Avoid a "." (period) in footprint names.
  • Avoid package names containing Microsoft®Windows® reserved words. For example, Con, Nul, Aux Prn, etc. Otherwise the translator cannot create the required device file (.txt).
  • Important; Cadence recommends running Tools -Derive Connectivity (derive connectivity command) Tools - Database Check (dbdoctor command) and Tools - Padstack - Modify Design Padstack (padeditdb command) before opening your translated Allegro PCB Editor design.