For OrCAD users who want to mill their circuit board designs on the Bantam Tools™ Desktop PCB Milling Machine, here are instructions to generate Gerber files that can be imported into Bantam Tools™ Desktop Milling Machine Software.
What is OrCAD?
Where do I get OrCAD?
Where can I find documentation about OrCAD?
You can find OrCAD’s resource library here.
How do I get my board from OrCAD into Bantam Tools™ Desktop Milling Machine Software?
You’ll need to configure OrCAD to export Gerbers and NC Drill Files in a format that the software 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 the software 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 the software
- In the software, click the Open Files button.
- Navigate to the directory that contains your Gerber files.
- Open TOP.gbr. (It if still has the .art extension, rename to .gbr.)
- 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.
- Click Okay to finish opening the files.
Import dialog with all files selected.