Documentation

Importing OrCAD Files

5 min read

OrCAD files in the following formats can be opened in Pulsonix:

  • OrCAD PCB designs and libraries in the MIN ASCII format for versions 7.2 through to 10.0, .brd (Binary) format for versions 16.x to current and Schematic designs and libraries in Edif ASCII format.

  • Design types supported are for:

Schematics and PCB

  • Library types supported are for:

Schematic Symbols and PCB Footprints, and Parts libraries

Exporting Schematic designs From OrCAD

To Export a Schematic design file from OrCAD

  1. From the File menu option in OrCAD Capture select Open and then Design
  2. Choose the DSN file which contains the Schematic design that you want to export.
  3. Select Export from the File menu.
  4. Choose the EDIF tab
  5. Type in or Browse the name that you want to save it as.
  6. It is recommended that you use the standard cap2edi.cfg configuration file that is supplied with Capture.
  7. Select OK to export the EDIF ascii file.

Note that the extension for schematic design Edif files is .edf as opposed to .edn for OrCAD Native EDIF netlists.

Exporting Parts and Schematic Symbol Libraries From OrCAD

The Schematic symbol and Part data are held within the same Library.

Please note that due to a limitation in the OrCAD Library Edif format, Part aliases cannot be handled.

To Export a Part/Symbol library file from OrCAD

  1. From the File menu option in OrCAD Capture select Open and then Library
  2. Choose the OLB file which contains the Schematic symbols and parts that you want to export.
  3. Select Export from the File menu.
  4. Choose the EDIF tab
  5. Type in or Browse the name that you want to save it as.
  6. It is recommended that you use the standard cap2edi.cfg configuration file that is supplied with Capture.
  7. Select OK to export the EDIF ascii file.

Exporting PCB designs From OrCAD version 16.x to current

Note: You will require the Allegro Importer option activated on your license for this process.

OrCAD PCB designs can be imported into Pulsonix using the OrCAD supplied extracta.exe which produces an ASCII version of the OrCAD design. You must have OrCAD installed on your system for this to work.

Setting Up the OrCAD Importer

In order to import OrCAD files, you will need to set up the extracta.exe path which is supplied with OrCAD/Allegro. To do this, from within Pulsonix go to the Tools menu, Options, General, click browse on the Allegro Extract File Path section and browse to your extracta.exe. This is likely to be in the tools\pcb\bin sub folder of your Allegro or OrCAD installation.

Once you have defined the path to the extracta.exe you can now open the Allegro files from within Pulsonix, as explained below.

Reading OrCAD files into Pulsonix

In Pulsonix, use File | Open to browse and open an OrCAD/Allegro board (.brd) file.

Exporting PCB Footprints from OrCAD 16.x to current

OrCAD/Allegro does not provide PCB Footprint Libraries in an ascii format. In order to read in the PCB Footprints, open the Library Manager and on the PCB Footprints tab, click the Import button. Now point to the OrCAD/Allegro .brd file.

Importing OrCAD Netlists into Pulsonix PCB

If using OrCAD Schematic Capture as your choice of Schematic design editor, you can export a netlist which can be read into Pulsonix PCB. (This is not the same as a full graphical Schematic export from OrCAD which will rebuild the whole Schematic design in Pulsonix).

Pulsonix PCB can accept OrCAD netlists in the following formats:

  • OrCAD Native EDIF netlist (*.edn) format, or;
  • OrCAD PCB 386 (*.NET) format.

To Import a netlist file from OrCAD

  1. Use the File menu and Import Design Data option to import your OrCAD netlist.
  2. During import, if the imported file contains components or packages not yet defined in any internal mapping, Pulsonix produces a report containing the omissions. You should use this report to correct problems in OrCAD. You have access to a Mapping file to map Parts or Footprints.
  3. Once imported, use the Import ECO option from the File menu to import subsequent changes with minimum impact on the existing PCB design.

Exporting data from OrCAD 7.2 to 10.0

OrCAD 7.2 to 10.0 designs and libraries are held in a binary format. The designs and libraries must be exported to the appropriate ASCII format.

To Export a PCB design file from OrCAD

  1. From the File menu option in OrCAD Layout select Export and then Min Interchange
  2. Choose the MAX file which contains the PCB design that you want to export.
  3. Save it as the name that you want to call the ASCII file.

Exporting PCB footprints From OrCAD

  1. From the File menu option in OrCAD Layout select Export and then Min Interchange
  2. Choose the LLB file which contains the PCB footprints that you want to export.
  3. Save it as the name that you want to call the ASCII file.

Open | Import Netlist | Data Transfer Wizard

Backlinks