If you use Altium and you’d like to mill circuit boards on the Bantam Tools™ Desktop PCB Milling Machine, you’ve come to the right place. This guide will give you tips on designing PCBs for the milling machine, as well as describe the process of generating Gerber and NC Drill files from Altium, which can then be fabricated on the milling machine.
Designing PCBs for the Bantam Tools™ Desktop PCB Milling Machine
Designing for our milling machine is different than designing for a PCB manufacturer. We strongly recommend reading our PCB Design Considerations guide first, but here are some highlights:
- The Mechanical 1 layer must contain the board outline, drawn with the Line tool. This is required for Otherplan to understand the size and shape of the board outline.
- 10 mil minimum trace and space for Othermill, 6 mil for the Bantam Tools™ Desktop PCB Milling Machine and Othermill Pro
- 10 mil minimum annular ring for Othermil, 6 mil for the Bantam Tools™ Desktop PCB Milling Machine and Othermill Pro
- Vias are not plated (meaning they aren't electrically conductive), so you need to solder a wire or rivet on both sides of the board
- Through-holes are not plated, so avoid routing traces to the top side of inaccessible through-hole pins
- If you’re using polygon fill / a ground plane, set your isolation value to 0.001"-0.002" larger than largest tool you want to use. Larger values will allow you to use larger tools, which will speed up your milling time.
- Slotted/oval holes are not supported. If you need them, make a row of overlapping holes that are a few thousandths of an inch larger than the tool and overlapping by about half their diameter (i.e. for a 1/32" (0.031") tool, make a row of 0.033" holes, with centers spaced 0.016" apart).
How do I get my board from Altium into Bantam Tools™ Desktop Milling Machine Software?
To get your PCB design from Altium into the software, you’ll need to export Gerber and NC Drill files. You can then import those files into the software, the software that controls the milling machine.
The layers you’ll need to export from Altium are:
- Top copper layer
- Bottom copper layer (if your board is double-sided)
- Mechanical layer to serve as the board outline
- NC Drill file for your drills/holes
Now that you know what you’ll be exporting, you can use our output job file to do it automatically! Download the output job file here or at the bottom of this page. It will generate the above output files and put them in a Project Outputs folder inside your Altium project folder.
Generating Gerber files using an output job
- In Altium, right-click on a project’s entry in the Projects panel.
- Choose “Add Existing to Project” and locate the output job.
- Expand the Settings folder and then the Output Job Files folder under your project.
- Double-click the output job to open it.
- Within the output job, select both the Gerber and NC Drill outputs, and then hit F9, which will generate the files in an Output folder inside your project folder.
Output job file open with Gerber and NC Drill outputs selected.
Check out Altium’s documentation if you’d like more information on making your own output jobs.
Generating Gerber files manually
As an alternative to using output jobs, you can also create Gerber and NC Drill files manually via File Menu > Fabrication Outputs. Here are a few things to keep in mind:
- Use 2:3 as your format, since the the machine's precision is 1 mil.
- Make sure you use the same format for both the Gerber and NC Drill files (Altium sometimes will use different formats by default).
- Uncheck all the “Other” options (G54, optimize change location commands, etc.).
- Choose “Separate file per layer” under Batch Mode for the Gerbers.
The other settings (leading/trailing zeroes, absolute vs relative, etc.) don’t matter as long as they’re the same between the Gerber and NC Drill files. Here are some screenshots of the Gerber configuration pages:
Once your Gerber and NC Drill files have been generated, you’re ready to switch to the software and import your files.
Import your Gerber files into the software
- In the software, click the Open Files button.
- Navigate to the directory that contains your Gerber files from Altium.
- Open the Gerber file containing the Top Copper layer (usually ends in .gtl)
- In the resulting dialog, check that the correct files are selected for the Outline (needs a .GM1 or .GKO file) and Holes (needs the .TXT file generated by the NC Drill output). See the screenshot below for an example.
- Click Okay to finish opening the files.
Import dialog with all files selected.
Import your Gerber files into our software:
- In the software, click the Import Files button.
- Navigate to the directory that contains your outputs from Altium.
- Click once on the top copper layer Gerber to select it.
- Look in the bottom pane of the window and make sure the associated files (bottom copper, board outline, and drills/holes) are selected. If they are not, select them from the dropdown menus.
- Click Import to complete the import process.