For OrCAD users who want to mill their circuit board designs on the Othermill, here are instructions to generate Gerber files that can be imported into Otherplan.

What is OrCAD?

OrCAD is a commercial app suite for designing circuits, made by Cadence. OrCAD PCB Designer is the program within the suite used to design circuit boards. OrCAD runs on Windows only.

Where do I get OrCAD?

A Lite version of OrCAD is available here. The commercial version is available through OrCAD distributors.

Where can I find documentation about OrCAD?

You can find OrCAD’s resource library here.

How do I get my board from OrCAD into Otherplan?

You’ll need to configure OrCAD to export Gerbers and NC Drill Files in a format that Otherplan can understand. To do so, follow these instructions. These instructions were tested on OrCAD PCB Designer Lite 17.2-2016. Settings and screenshots may differ for other versions.

  • In OrCAD PCB Designer, click Export > Gerber.
  • In the Gerber Parameters tab, make sure that the following options are selected:

    • Gerber RS274X: Selected
    • Output Units: Inches
    • Integer Places: 2
    • Decimal Places: 4
    • Leading Zeros: Deselected
    • Trailing Zeros: Deselected
    • Equal Coordinates Zeros: Deselected


  • In the Film Control tab, right-click the TOP film (it has a folder icon) and select Add Manual.
  • Enter “OUTLINE” for the film name and click OK.
  • In the Available Subclasses window that appears, click the plus icon to expand the BOARD GEOMETRY class, check the boxes next to DESIGN_OUTLINE and CUTOUT, and click OK. (Depending on your design, you may need to select OUTLINE as well.)


  • Check the boxes next to BOTTOM, OUTLINE, and TOP.
  • Click Create Artwork to generate Gerbers. These will be created as TOP.art, BOTTOM.art, and OUTLINE.art. You will need to rename these to have a .gbr extension so that Otherplan will load them.


If your board has holes, you’ll also need to export an NC Drill file:

  • Click Export > NC Drill.
  • In the NC Drill window, select the following settings:

    • Auto tool select: selected
    • Separate files for plated/non-plated holes: deselected


  • Click the NC Parameters button.
  • In the NC Parameters window, enter the following settings:

    • Format: enter 2 in the first box and 4 in the second
    • Leading zero suppression: deselected
    • Trailing zero suppression: deselected
    • Equal coordinate suppression: deselected
    • Enhanced Excellon Format: selected


  • Click Close.
  • Click Drill to generate the drill file.

Import your Gerber files into Otherplan

  1. In Otherplan, click the Open Files button.
  2. Navigate to the directory that contains your Gerber files.
  3. Open TOP.gbr. (It if still has the .art extension, rename to .gbr.)
  4. In the resulting dialog, ensure the correct files are selected for the Bottom (if you’re milling a double-sided board), Outline, and Holes (ends in .drl). See the screenshot below for an example.
  5. Click Okay to finish opening the files.


Import dialog with all files selected.