« home

Milling a PCB with Auto-Leveling using a Carbide 3D Nomad 3

I tried everything between Carbide Copper, which seems abandoned at best and buggy at worst: it does not seem to spin the spindle. I played with FlatCAM and bCNC, which I used to brick my Nomad 3. (I provide instructions to reset the GRBL on a Nomad 3, much thanks to Carbide 3D support.)

Ultimately, I settled on pcb2gcode for generating G-code and coppercli for copper milling. coppercli is a cross-platform keyboard-driven CLI, originally based on OpenCNCPilot.

Example Results

PCB Soldered PCB Top view

Video: Probing

Acknowledgements

Chris Kohlhardt's notes partly inspired this work. He uses FlatCAM and bCNC. I found both rather inscrutable. Much thanks to Martin Pittermann for OpenCNCPilot, which coppercli is based on, and for the feedback. Thank you to deHarro. Much thanks to Eyal for pcb2gcode.

CNC Machine

This has been tested on a Carbide 3D Nomad 3 CNC Mill.

coppercli logo coppercli

coppercli is a cross-platform (Mac, Linux, Windows, and web) tool for PCB milling on GRBL machines with probe-based auto-leveling, tool changes, real-time visualization, depth-adjusted remills, session recovery, and a safety-first approach. Originally based on OpenCNCPilot.

PCB Blanks / Copper Clad

First of all, and most importantly: DO NOT USE FR4 copper clad in a CNC machine. Only ever use FR1 copper clad. Glass fiber dust is an extremely dangerous health hazard.

I use 2x3" and 4x6" PCB blanks that I order from Carbide 3D. I have also used 100x150mm and 150x200mm PCB blanks. They are single-sided ("SS") or double-sided ("DS") and are also sold on Amazon and AliExpress. As mentioned above, only use FR1 copper clad, NEVER USE FR4.

You'll likely start with your entire PCB on one (the non-copper) side and soldering the pins on the copper side, so you need single-sided copper clad.

If you plan to put the ground plane on the opposite side, you will need double-sided copper clad. However, I have not yet found a good way to work with double-sided copper clad. Remember that plugging in pins through double-sided copper clad will connect the pins on both sides of the board, even if you only solder one side. The edges of the pin will very likely make contact with the copper. I learned this the hard way.

Drill/Mill Bits

V-bits in 30°, 40°, and 60° angles.

30° V-bits

40° V-bits

60° V-bits

Jigs

I provide several different-sized jigs on printables.com. Please be in touch if you need additional sizes. If you do not have access to a 3D printer, I can print them and send them to you for $49.99 plus shipping. Others can do it, no doubt, for much less.

BitZero Attachment

You need to rig the BitZero V2. Anything works as long as it conducts ground between the top of the copper clad and the BitZero. This is my solution.

BitZero rig

Workflow Outline

  • Adjust the PCB design.
  • Export Gerber files.
  • Attach copper to the jig with double-sided tape.
  • Zero X, Y, Z.
  • Probe to create a height map. This can take 15-30 minutes, depending.
  • Mill front (for example, using a 30° V-bit). This can take 30m-3h hours, depending.
  • [Optional: flip, mill other side, flip back]
  • Replace V-bit with a drill bit (for example, a 0.8mm PCB drill).
  • Zero Z.
  • Drill holes.
  • Drill outline.
  • Prepare to solder.
  • Solder.

If you are milling both sides, you should drill after milling both sides; otherwise, you are level-probing a surface with holes.

Single-layer Design on B.Cu

This tutorial assumes you are making a single-layer PCB where you plug in components at the top and solder them at the bottom. This means your entire PCB design needs to be on B.Cu.

If you initially designed your board for manufacturing (e.g., JLCPCB, PCBWay, OSH Park, etc.), you likely put the GND plane on B.Cu and the signal traces on F.Cu. That will not work for CNC manufacturing. (I discovered this the hard way when all my pin holes were mirrored.)

To adapt the design for CNC manufacturing, you need to move all routing (including GND) to F.Cu. Since GND is no longer taken care of, this likely requires re-routing traces.

While you are at it, you need to also make the tracks wider and clearance wider:

KiCad margins

Using File → Board Setup → Design Rules → Net Classes:

Using File → Board Setup → Board Stackup → Physical Stackup:

If you change this, you need to apply your changes using Edit → Edit Track and Via Properties → select Set to net class / custom rule values and Apply. Then run the Design Rules Checker and fix any errors due to the width changes. People have reported thinner track widths, though.

Once everything is on F.Cu, you can swap F.Cu and B.Cu (using menu Edit → Swap Layers...) to transpose F.Cu to the back. Alternatively, if you are not planning to use a PCB manufacturing service, you can do all routing on B.Cu from the start.

Check Your PCB

This is obvious, but my most frequent mistakes are incorrect rotation of pin headers and misalignment of pins. Hold the parts you will use to the screen. It sounds silly, but holding them next to each other is a great way to find bugs. Check pin assignments. Use the measuring tool in KiCad to check distances between pins (typically multiples of 2.54mm) and alignment. Measure the distance between the physical pins with a caliper to verify your PCB design. (Alternatively, use the Snap To Grid function in the pcb-action-tools plugin to do this automatically.) And, of course, Run DRC and fix all Violations and Unconnected items.

KiCad PCB Export

A few things to keep in mind when exporting from KiCad's PCB editor:

KiCad origin

KiCad Plot / Export

Using menu File → Plot...:

KiCad plot

Press "Plot".

Then:

Then press "Generate".

KiCad drill

Back on the Plot window, press "Plot"

Generate G-code from .gbr Files

Using pcb2gcode and the millproject configuration file.

Create a file millproject in the same directory as the .gbr files.

# See https://github.com/pcb2gcode/pcb2gcode/wiki/Manual

metric=true
metricoutput=true

# milling
zwork=-0.06          # Depth in mm; -0.06mm and -0.07mm work well for me
zsafe=20             # Height for movements; start with 20mm, can be 1mm if confident
# zsafe=1            # Height for movements; start with 20mm, can be 1mm if confident
zchange=35           # Height for tool changes
mill-feed=100        # Feed rate in mm/minute; can go up to 600, or even 800.
                     # That will DRAMATICALLY speed up the milling process at the price
                     # of slightly more granular cuts.
mill-speed=12000     # RPM for milling; can go up to 14000 or even 16000
nom6=1               # Suppress tool changes; pcb2gcode-wrapper --multi handles them
spinup-time=3.0      # Time to spin up the spindle in seconds
spindown-time=3.0    # Time to spin up the spindle in seconds
backtrack=1          # Allow retracing through existing path; speedup
isolation-width=0.6  # As thick isolation as possible without running into trouble
milling-overlap=25%  # Re-mill with 25% overlap as part of creating isolation width

# Voronoi regions
voronoi=1            # Try it out! Makes soldering easier, but looks funky; default 0
# min-path-length=0.1 # Not yet in the official release, currently in MR

# drilling
zdrill=-1.7          # Drill depth; measure your copper clad
zmilldrill=-1.7      # Mill drill depth; measure your copper clad
drill-feed=100       # Feed rate in mm/minute; can go up to 200
drill-speed=12000    # RPM for drilling; can go up to 14000
nog81=1              # Use G0/G1 instead of G81/G80; required for coppercli
drills-available=0.8 # Your 0.8 drill bit
min-milldrill-hole-diameter=0.81 # Milldrill anything greater than 1mm
milldrill-diameter=0.8 # Same drill bit as drilling

# outline cutting
zcut=-1.7            # Cut depth for outline; same as drill depth
cut-feed=100         # Feed rate for outline cutting; same as milling
cut-vertfeed=60      # Vertical feed rate; similar to drill-feed; can go up to 20
cut-speed=16000      # RPM for cutting; same as mill-speed
cutter-diameter=0.8  # Diameter of end mill for cutting (in mm)
bridgesnum=0         # No bridges; it's stuck with tape
cut-infeed=0.4       # Max cutting depth per pass

# this will mess up offset! don't use!
# zero-start=true

Some of these values are critically important:

  • zsafe is the travel height of the mill bit; if this is too low your bit will crash into the jig, breaking the mill or worse. Once you get the hang of it, you can make this as low as 2.
  • zchange is the height for changing the mill bit; if you choose this number too high and your drill bit is long, the process will error out, because it runs into the hard limit of the machine.
  • zwork is how deep the mill drills into the copper substrate; start with 0.05 and iterate deeper as needed; this also depends on the V-bit you are using.
  • nom6=1 suppresses tool change commands in individual files. Instead, pcb2gcode-wrapper --multi adds tool changes when combining files, giving us control over when and how tool changes happen.
  • nog81 prevents pcb2gcode from issuing G81 commands, which trips up OpenCNCPilot.
  • For --mill-diameters you can use this tool cutting width calculator to figure out the correct number.
  • Once you're comfortable with the process, you can dramatically speed it up by increasing values marked "can go up to" in the comments above: mill-feed, mill-speed, drill-feed, and drill-speed. Higher speeds mean faster operation but may produce slightly rougher cuts.

Run pcb2gcode to generate the back, which, confusingly, is what we're going to mill.

# replace "decibel-meter-B_Cu.gbr" with your own .B_Cu file
# optional: --basename FOO to give file a nice prefix
# optional: --output-dir DIR to write file to another directory
# optional: --x-offset negative number moves the PCB to the right of the origin
#           this should equal the width of your board
# --mill-diameters: the width of your mill at the given zwork
pcb2gcode --back decibel-meter-B_Cu.gbr --mill-diameters=0.169

Generate the Excellon drill file:

# replace "decibel-meter-PTH.drl with your own .drl file
# optional: --basename FOO to give file a nice prefix
# optional: --output-dir DIR to write file to another directory
# optional: --x-offset negative number moves the PCB to the right of the origin
#           this should equal the width of your board
#           MAKE SURE THIS IS THE SAME AS THE SETTING FOR B_Cu ABOVE
pcb2gcode --drill decibel-meter-PTH.drl --drill-side back

Generate the outline file:

# replace "decibel-meter-PTH.drl with your own .drl file
# optional: --basename FOO to give file a nice prefix
# optional: --output-dir DIR to write file to another directory
# optional: --x-offset negative number moves the PCB to the right of the origin
#           this should equal the width of your board
#           MAKE SURE THIS IS THE SAME AS THE SETTING FOR B_Cu ABOVE
pcb2gcode --outline decibel-meter-Edge_Cuts.gbr --cut-side back

Alternatively, install my pcb2gcode-tools package:

brew install pipx
pipx install git+https://github.com/thomergil/pcb2gcode-tools

Then run pcb2gcode-wrapper, which invokes all three scripts with the same parameters, automatically calculates offsets from your Edge_Cuts.gbr file, and post-processes the output:

$ pcb2gcode-wrapper decibel-meter --mill-diameters=0.169

The wrapper automatically calculates the --x-offset from the board width: x-offset = -1 * (ceil(width_mm) + x_margin). The default x_margin is 5mm. The --y-offset defaults to 3mm (the y_margin value). You can override these defaults:

$ pcb2gcode-wrapper decibel-meter --mill-diameters=0.169 --x-margin 10 --y-margin 7

The wrapper automatically runs pcb2gcode-fixup (swaps initial XY/Z moves for safety) and pcb2gcode-combine (merges drill/milldrill/outline into a single file when they use the same bit).

For a single-file workflow with automatic tool changes, add --multi:

$ pcb2gcode-wrapper decibel-meter --mill-diameters=0.169 --multi

This creates an additional _000_all.ngc file that combines milling and drilling with automatic tool change pauses. When you run this file in coppercli, it will pause at each tool change, guide you through swapping bits, and re-zero Z using the tool setter (if configured) or manual probing.

Either way, you should now have .ngc files.

Attach Copper Clad to Jig

Cover the entire bottom surface of the copper clad (all the way to the edges) with non-overlapping double-sided tape. Don't just tape the middle because the sides will flex downward during probing.

Double-sided tape

Then press the copper clad into the jig with a paper towel:

Copper clad in jig

coppercli logo Milling with coppercli

coppercli is a cross-platform (Mac, Linux, Windows, and web) tool for PCB milling on GRBL machines with probe-based auto-leveling, tool changes, real-time visualization, depth-adjusted remills, session recovery, and a safety-first approach. Originally based on OpenCNCPilot. See the coppercli README for installation instructions and full documentation.

General Notes

coppercli and Carbide Motion Don't Play Nice

Switching to coppercli after using Carbide Motion is usually OK. However, using Carbide Motion after coppercli can fail in mysterious ways, starting with initialization and homing. Stay close and keep your finger on the power button. If weird things happen, follow my instructions to reset the GRBL on a Nomad 3.

Start coppercli

Run coppercli from the command line. On first run, go to Settings and select your Machine Profile (e.g., Nomad 3). This configures the machine-specific tool setter position.

From the main menu, choose Connection. coppercli will auto-detect your serial port and baud rate. Once connected, it will offer to home the machine.

If it's not working: reset the machine, restart coppercli. Make sure the door magnet is engaged.

Load the G-code

Choose Load G-Code and browse to the .ngc file generated by pcb2gcode.

Set the Zero Point for X and Y (but Z comes later)

Choose Jog to enter the Jog menu. Use arrow keys to jog the spindle. Press Tab to cycle through speed presets—start with Fast, then switch to Slow or Creep as you get close.

Move the mill bit to the bottom left corner of the copper clad. Ensure that you set the zero point slightly away from the clip [see image below].

Zero point

Lower the bit to roughly 2mm above the surface using Page Down. Then press P to Probe Z—the bit will probe down until it touches the copper. The photo below shows the BitZero light turned red, confirming successful contact.

Probe contact

Once the probe completes, press 0 to Zero All (XYZ).

Probe the Surface

Choose Probe from the main menu. You'll be prompted to enter:

coppercli then creates the probe grid using the bounds of your G-code file plus the margin you specified.

Run Probe

Choose Start Probing. You'll be asked: Trace outline first?

Trace outline: Before probing, the spindle will move around the outer boundary of the probe area. You'll be prompted for a trace height and feed rate—choose a height where you can visually verify that the spindle stays within the copper clad. Watch the trace carefully. If the spindle goes past the edge of your copper, press Escape to cancel and reposition your work zero before probing begins.

After the trace, probing begins. The mill will lower until it touches the surface, then visit all probe points. A visual matrix shows progress with color-coded heights indicating surface variation.

After tracing, coppercli starts probing and creates a colorful heightmap. Red is high, blue is low.

Probing

Press Escape at any time to stop. coppercli auto-saves progress, so you can resume an interrupted probe session later.

Remove All Hardware

Remove all the hardware from the CNC. Carefully remove the alligator clip without pulling on the copper clad.

Apply Probe Data and Mill

After probing completes, coppercli will prompt you to apply the probe data to the G-code and proceed to milling. The milling screen shows progress, position, and ETA.

Milling screen

Tool Changes (milling → drilling → outline)

If you used --multi to create a single _000_all.ngc file, coppercli handles tool changes automatically. When a tool change is needed, coppercli will:

  1. Pause and display which tool to load
  2. Move to an accessible position for bit swapping
  3. Wait for you to change the bit and press Y to proceed
  4. Automatically re-zero Z using the tool setter (if configured in Settings → Machine Profile)
  5. Resume milling with the new tool

If you don't have a tool setter configured, coppercli will prompt you to manually probe the surface with the new bit.

Flipping the Board (double-sided PCBs)

If you flip the board for double-sided milling, you must re-zero and re-probe:

Soldering

Soldered PCB

Back to top