This guide shows you how to export your PCB designs from CircuitMaker as Gerber files that can be imported into Bantam Tools Milling Machine Software and milled on your Bantam Tools Milling Machine mill.
What is CircuitMaker?
CircuitMaker is a free electronic design automation software package and online project community for hackers, makers, and the like. It’s made by Altium, which is known for its professional EDA software package, Altium Designer. CircuitMaker is nearly the same as Altium Designer, but it has the caveat that all your designs are stored publicly in the Community Vault. You must also be connected to the internet in order to use CircuitMaker.
You can download CircuitMaker on the site.
Designing PCBs for the Milling Machine
Designing a PCB for the milling machine is a little different than designing for a PCB manufacturer. Here are some design considerations:
- 10 mil minimum trace and space
- 10 mil minimum annular ring
- Through-holes are not plated, so avoid routing traces to the top side of inaccessible through-hole pins.
- Vias are not plated, so you’ll need to solder a wire on either side of the board to connect vias.
- If you’re using polygon fill/a ground plane, set your isolation value to 0.001"–0.002" larger than the 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. For example, to make slots with a 1/32" (0.031") tool, make a row of 0.033" holes, with centers spaced 0.016" apart.
- The Outline 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.
We recommend setting your CircuitMaker design rules to match the milling machine design considerations so that your design process runs smoothly and your PCBs are fully able to be milled on the milling machine.
How do I get my board from CircuitMaker into Otherplan?
Export the following three layers as separate Gerber files, plus an NC Drill file:
- Top layer
- Bottom layer (if your board is double-sided)
- Outline layer to serve as the board outline (requires lines drawn on the Outline layer)
- NC Drill file for your drills/holes
You can then import those files into Otherplan, the software that controls the milling machine. See below for more detail on generating Gerber and NC Drill files.
Exporting CircuitMaker Designs as Gerber and NC Drill Files
Step 1: Start the process of generating output files. In the Ribbon under the Home tab, open the Project menu and click Generate Outputs.
Step 2: Click OK when prompted to save and commit your files.
Step 3: In the Generate Output Files dialog, check the boxes for Gerber Files and NC Drill Files.
Step 4: Click the Configure link next to Gerber Files. In the dialog that opens, configure the following options in the General tab:
- Use 2:3 as your format, since the milling machine’s precision is 1 mil. You can use a higher format if you want, but it won’t make a difference in how it’s milled. Inch vs. millimeter also doesn’t matter to Otherplan.
- Remember what setting you choose here because you’ll need to use the same settings when you configure your NC Drill files.
Step 5: In the Layers tab, check the boxes for Top Layer, Bottom Layer (if your board is double-sided), and Outline. Don’t check any of the boxes in the panel on the right.
Step 6: In the Advanced tab (skip Drill Drawing and Apertures), configure the following options:
- The Film Size and Aperture Matching Tolerance settings don’t matter to Otherplan, so you can ignore them.
- Uncheck all the “Other” options (G54, optimize change location commands, etc.)
- Choose “Separate file per layer” under Batch Mode for the Gerbers.
- For advanced settings like leading/trailing zeroes, vector/raster, and absolute/relative, it doesn’t matter to Otherplan as long as you use the same settings when you configure the NC Drill setup.
Step 7: Click OK to return to the Generate Outputs dialog, then click the Configure link next to NC Drill Files. Configure the following settings in the NC Drill Setup dialog:
Step 8: Click OK to close the NC Drill Setup dialog.
Step 9: In the Generate Output Files dialog, click the Generate button. You’ll be prompted to save a zip file of the generated files. Choose a location and click OK.
Step 10: Unzip the saved file, go into the NC Drill folder, and drag the .txt file from the NC Drill folder into the Gerber folder. You should have the following highlighted files together in the same folder. It ultimately doesn’t matter where they are as long as they’re together.
Congrats! You’ve successfully exported your CircuitMaker design as Gerber files and you’re ready to import them into Otherplan and mill them on the milling machine.
Importing Gerber Files into Otherplan
Step 1: In Otherplan, click Open Files.
Step 2: Navigate to the folder containing your Gerber and NC Drill files.
Step 3: Select the GTL file and click Open.
Step 4: In the Gerber Import dialog, make sure that your Outline, .gbl (if your board is double-sided), and .txt files are selected for Outline, Bottom Copper, and Drills/Holes. Then click OK.
Step 5: Your design will be displayed in Otherplan as a simulation on the left and a plan panel on the right. Set your board dimensions if they’re different than the defaults, and choose the tools needed to mill your board (determined by the minimum spacing between traces and components).