CNC Milling Circuit Boards
I finally was able to mill a circuit board using my CNC machine. No more acid etching, but I never had much luck with it anyways. After milling the table and fixture, I was held up by the lack of 1/8″ collet, which Bosch doesn’t make. I bought a nice collet set from Think & Tinker/PreciseBits for a modest price and it seems it was worth it. I also needed to buy a license for Mach3 to go beyond the 500 line code limit, since the code to etch the board was near 20,000 lines. To produce the G-code from an EagleCAD project, a nice script is available for free, http://www.pcbgcode.org/. It installs like any other ULP script for EagleCAD and comes with docs to get you going, plus forums and plenty of other websites with tutorials.
It was neat watching the CNC machine cut the traces and no broken bits or other catastrophes. Unfortunately, I didn’t take the time to properly zero the end of the 45 degree v-bit and cut too deep. This washed out the traces and pads, so it’s scrap. Before I realized this though, I tried fiddling with the settings for the pcb-gcode script and kept milling on the sheet of copper clad board and got a lot more bad traces.
The correct way to zero the end of the tool was to use a piece of paper between the board and the tool and to jog down at a very low speed (about 3% of max). While the tool is going down, move the paper back and forth till the tip catches it. Now zero the Z-axis in the Offsets tab of Mach3 in one of special G-code offset codes of your choice. Then measure the thickness of the paper with calipers (my piece was .0035″) and subtract it from the Z offset (press the “Save Work Offset” button to bring up a dialog box that allows you to edit the coordinates). This puts the Z-axis 0 coordinate on top of the circuit board without any pressure. The X & Y coordinates are set to where you want to start milling the board, and can be done by eyeballing it, just don’t re-zero the Z-axis. Now the machine is set to mill.
My settings for pcb-gcode script (not all are included, just what I changed):
Default = .0001″
Maximum = .0001″
Step Size = .005″
Etching Tool Size = .007″
Z High = .5″
Z Up = .1″
Z Down = .002″ (someone posted an excel file in the pcb-gcode forums to calc this, I set mine .001″ higher and it worked)
Drill Depth = .065″ (go a little deeper than the board thickness)
X = 0
Y = 0
Z = .5″ (don’t leave as 0 or the machine will drag the end of the drill bit across the board between tool changes)
XY = 10″/min
Z = 5″/min
Change any other options you need, then hit “Accept and make my board”. All the files generated will be placed in the project folder with the board. Check out the readme file in the docs folder for explanations, it was helpful. I’ll probably try setting the Maximum Isolation setting to something higher, so the slivers between close traces are removed. I’m sure I’ll update with more progress, or at least to show of stuff I made.