A class guide for cutting non-ferrous metals on the Nomad 3 desktop CNC.
Prerequisite: This builds on the X-Carve CNC Router Badge. You should already be comfortable with CNC vocabulary, zeroing, toolpaths in VCarve (or Fusion), and running a job in either OpenBuilds or Masso CONTROL before working through this page. We won't re-cover any of that here. View CNC Router Class Curriculum Here >
Big idea: The Nomad 3 is a rigid little machine, but it is still a desktop mill. Metal cuts well on it when you respect the limits: shallow depths of cut, the right tool, and good workholding. Push past those limits and you get broken endmills, chattery surfaces, and pulled-up parts.
Good news: the software workflow for the Nomad is the same one you already know.
Cutting Metal on the Nomad 3 — YouTube
It covers a lot of the same ground discussed below. If you only have time for one resource, watch this before getting started.
Sorted from easiest to hardest. Start at the top of the list and work your way down only after you're comfortable.
The friendliest metal for a desktop CNC. 6061-T6 is the standard go-to — it machines cleanly, is widely available, and is very forgiving. Avoid pure aluminum (too soft and gummy) and high-silicon casting alloys (abrasive, hard on tools).
Honestly, brass is also very beginner-friendly. Many people find it easier than aluminum because the chips break instead of stringing. 360 brass ("free-machining brass") is the gold standard.
Doable but trickier than brass. Copper is gummy. it likes to grab the tool. Use sharper tools, more positive geometry, and don't dwell.
Carbide 3D says yes. We don't recommend it.
On paper, the Nomad 3 spec sheet lists mild steel as a supported material, and a handful of people on the forums have pulled it off with very light cuts, mist coolant, and a lot of patience. But this is a small desktop machine with a small spindle, and steel really wants more rigidity and torque than it has. Realistically you'll get chattery surfaces, broken tools, and very long cycle times and it's not a good experience for a beginner. We want you to like milling!
If you need to cut steel, this isn't the machine for it. For this class, stick to aluminum, brass, and copper.
For non-ferrous metals (aluminum, brass, copper), use a 2-flute or 3-flute endmill.
Coatings matter too. For aluminum, use uncoated or ZrN-coated carbide. Do not use TiAlN/AlTiN on aluminum — the aluminum content in the coating makes aluminum love to stick to it.
For aluminum, brass, and copper on the Nomad 3: no, you don't need coolant.
Here's why:
For sticky materials (especially aluminum) you can wipe a stick lubricant (WD-40, kerosene, or a dedicated tap fluid like Tap Magic or Anchorlube) directly on the workpiece between passes. This is not coolant — it's just enough to keep chips from welding.
TL;DR on lube: Aluminum, brass, and copper → air blast is plenty.
These are starting points for the Nomad 3 with a 1/8" (3.175 mm) 2-flute carbide endmill. Always start conservative and dial up.
| Material | RPM | Feed rate | Depth of cut | Stepover |
|---|---|---|---|---|
| Aluminum 6061 | 10,000 | 20 in/min (500 mm/min) | 0.010" (0.25 mm) | 40% |
| Brass 360 | 10,000 | 15 in/min (380 mm/min) | 0.010" (0.25 mm) | 40% |
| Copper | 10,000 | 12 in/min (300 mm/min) | 0.008" (0.20 mm) | 35% |
A few notes on the numbers:
Where to actually get your feeds and speeds: buy your endmills from a reputable supplier — BitsBits, Harvey Tool, Helical, Datron, etc. — and use the conservative starting feeds and speeds they publish for that specific bit. Bit manufacturers know their own tools better than any generic chart will, and their numbers are usually tuned for hobby-grade machines. The table above is a fallback if you don't have manufacturer specs.
Workholding for metal is much more demanding than for wood or plastic. A part that comes loose mid-cut will break your endmill and can damage the machine.
Quick note on the Nomad's bed: the Nomad has its own aluminum fixture bed built in, with a grid of threaded inserts. Everything below either bolts directly into those inserts or uses the included step clamps that thread into them. You never screw through the bed itself — you screw into the threaded inserts that are already there, or you bolt a spoilboard/fixture on top of the bed and screw into that.
Here are your options, in order of what we actually have at the makerspace:
The makerspace has hold-down clamps that use T-track bolts: the T-bolt slides into a slot on the bed, and the clamp tightens down over the edge of your stock. This is what's available and what most projects will use.
A flat piece of MDF, plywood, or 6061 aluminum bolted to the Nomad bed via T-track bolts, with screws or more clamps holding your workpiece to the spoilboard. This is a great pattern because:
On going low-profile: A thinner fixture (say, 1/4" plywood or 1/4" aluminum) holds just as well as a thick one — the clamping force comes from the T-bolts pulling the fixture down onto the bed, not from the fixture's mass. The tradeoffs of going thin are: less thread for screws to bite into when you're securing your workpiece to the spoilboard, and less buffer before your profile cut reaches the actual bed. A 1/2" piece of MDF or plywood is the sweet spot for a class spoilboard — thick enough to profile through without worry, cheap to replace.
Works for shallow cuts in aluminum and brass — think engraving, light pocketing, name plates. Do not trust it for deep profiling. Surface prep matters: clean both surfaces with isopropyl alcohol, press hard, give it a minute to grip.
Surprisingly strong for thin material. Lay blue tape on the part and on the spoilboard, hit both with CA glue and accelerator, press together. Pops off cleanly with a chisel. Better than plain tape for small parts.
A dedicated Nomad low-profile vise is the best option for any part with a clean edge to grip — most repeatable, very secure. We don't have one at the makerspace right now. If enough students ask, we may add one; in the meantime, you're welcome to bring your own.
Great for production work. Soft jaws machined in-place give the best repeatability. Mentioned here so you know they exist if you go down the rabbit hole.
Same software as the X-Carve class — included here for reference. Pay special attention to the Probe Tool under Advanced & Maintenance, since you'll use it to zero on every metal part.
Best Practices:
Before you press Start on your first metal cut, run through this: