How to Cut Metal on a CNC Machine
This guide shows the working order we use on the shop floor: pick the tool, set the speeds and feeds, control the heat, and hold the part. It is written for engineers and buyers who need to judge whether a design can be cut well. When you cut metal on CNC machine setups, the order of decisions matters more than any single number.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
Key takeaways
What happens when you cut metal on a CNC machine
Cutting metal is a shearing process, not a grinding one. The cutting edge pushes into the workpiece, the material ahead of the edge deforms plastically, and a chip slides up the rake face. Almost all of the heat generated in that zone leaves with the chip. If it does not, the heat goes into the part and the tool, and both start to move.
That single idea explains most shop floor problems. A dull edge rubs instead of shears, so heat stays in the cut. A feed that is too light lets the edge skate over the surface and work-harden it. A tool that hangs too far out of the holder bends under load, changes the effective rake angle, and starts to chatter.
Three variables set the outcome: surface speed, feed per tooth, and radial and axial depth of cut. Surface speed comes from the tool substrate and coating. Feed per tooth comes from the chip load the edge can survive, which depends on edge radius and material hardness. Depth of cut comes from the rigidity of the whole loop: spindle, holder, tool, fixture, and part.
Before any of that, decide whether the feature should be milled at all. A deep slot narrower than 3 × tool diameter, a sharp internal corner, or a hole with a length-to-diameter ratio above 8 will cost more than the rest of the part combined. Sometimes the right answer is to change the drawing, not the cutting data.
Match the cutter to the metal before you cut metal on CNC machine jobs
Aluminum 6061 and 7075 cut cleanly with two or three flute carbide end mills, uncoated or with a ZrN coating. Run high surface speed, around 300 to 500 m/min, with a generous chipload. The risk is built-up edge on soft 6061, which shows up as a rough, smeared wall. A sharper edge and more feed fix it, not more speed.
Stainless 304 and 316 work-harden in front of the edge, so never dwell. Use a four or five flute tool with a positive rake and an AlTiN or AlCrN coating. Surface speed drops to roughly 60 to 120 m/min, and the feed per tooth stays high enough to keep the edge biting under the hardened layer. Too light a feed is the most common mistake here.
Steel 1045 and 4140 run at 100 to 180 m/min with coated carbide. Titanium Ti-6Al-4V is different: it conducts heat poorly, so the edge stays hot and the chip carries less away. Keep surface speed around 40 to 70 m/min, flood the cut with high-pressure coolant, and never let the tool rub. Inconel needs the same discipline with even lower speeds.
Plastics and copper alloys sit at the two ends. POM and PEEK cut fast but melt if the chip is not evacuated, so use a two flute tool with a polished flute and air blast. Copper and brass machine easily but grab the tool, so reduce rake angle and keep the flute count low to clear chips.
- 1Aluminum2–3 flutes, uncoated or ZrN, 300–500 m/min.
- 2Stainless4–5 flutes, AlTiN, 60–120 m/min, no dwelling.
- 3Steel4 flutes, coated carbide, 100–180 m/min.
- 4Titanium4–6 flutes, AlCrN, 40–70 m/min, high-pressure coolant.
Heat, chatter, and surface finish when you cut metal on CNC machine parts
Coolant does two jobs: it removes heat and it flushes chips. On aluminum, a mist or air blast is often enough because the chip carries most of the heat away. On stainless, titanium, and Inconel, use flood coolant or through-tool high-pressure coolant. The pressure matters more than the volume at the cutting edge.
Chatter is a vibration loop between the tool and the workpiece. It shows up as a rippled wall and a tone that changes with depth of cut. The fixes, in order of effect: shorten the tool, stiffen the fixture, reduce radial engagement, then change spindle speed. Changing speed alone rarely solves it.
Surface finish follows the tool nose radius and the feed per revolution on turning, and the stepover and tool runout on milling. For Ra 0.8–1.6 μm on aluminum, a sharp, low-runout tool with a 0.1 mm finishing stepover usually gets there. For Ra 0.2–0.8 μm, plan a separate finishing pass with a fresh edge and a light spring pass.
Burrs form wherever the edge exits the material. A 0.05 mm chamfer added to the drawing costs almost nothing and saves a manual deburring step. On stainless and titanium, a small edge break also reduces the risk of a sharp burr folding over and hiding a crack.
Step by step: how to cut metal on a CNC machine
Follow this order. Changing it usually means redoing the setup.
- 1Read the drawing for manufacturabilityMark every tolerance tighter than ±0.05 mm, every internal corner, and every deep pocket. Decide which features need a second op or a five-axis setup before you touch the machine.
- 2Choose the tool and holderKeep the tool as short as the geometry allows. Stick-out should not exceed 4 × diameter for roughing. Use a shrink-fit or hydraulic holder for finishing; a collet chuck is fine for roughing.
- 3Calculate surface speed and feed per toothTake surface speed from the tool and material table, convert to RPM with RPM = (1000 × Vc) / (π × D), then set feed = RPM × flutes × chipload. Start at 70% of the calculated feed for the first pass.
- 4Set depths of cutFor aluminum, rough at 50% of tool diameter radially and 1 × diameter axially. For stainless and titanium, drop radial engagement to 20–30% and use trochoidal paths to spread tool wear.
- 5Prove the setup with an air passRun the program 5 mm above the stock. Watch for holder collisions, check the tool change positions, and confirm the work offset moves in the direction you expect.
- 6Cut the first part and listenA steady hum means the chip load is right. A high-pitched squeal means too much speed or too little feed. A thumping sound means the part or fixture is moving.
- 7Measure while the part is still clampedCheck critical dimensions with the part in the vise. If it is out, you can still adjust the offset and recut. Once it is off the table, the setup is gone.
- 8Inspect and documentLog the tool, the parameters, and the measured result. The next run of the same part starts from those numbers, not from the chart.
Starting parameters by material
Ranges for coated carbide end mills with flood coolant. Adjust for tool stick-out and machine rigidity.
| Material | Surface speed (m/min) | Feed per tooth (mm) | Finishing note |
|---|---|---|---|
| Aluminum 6061 | 300–500 | 0.05–0.15 | Watch built-up edge; add feed, not speed |
| Aluminum 7075 | 250–400 | 0.05–0.12 | More rigid than 6061; holds thin walls better |
| Stainless 304 / 316 | 60–120 | 0.03–0.08 | Never dwell; keep the edge cutting |
| Steel 1045 / 4140 | 100–180 | 0.04–0.10 | Rough at 1 × D axial, 50% radial |
| Titanium Ti-6Al-4V | 40–70 | 0.03–0.07 | High-pressure coolant; low radial engagement |
| Inconel | 25–45 | 0.02–0.05 | Expect short tool life; plan for regrinds |
| Brass C36000 | 200–350 | 0.05–0.12 | Low rake angle; clear chips fast |
| POM / PEEK | 300–600 | 0.05–0.15 | Air blast; avoid melting the chip |
The rule we follow
Fix the setup before you chase the numbers. A rigid tool, a solid fixture, and a feed that keeps the edge cutting will beat any cutting data chart run on a weak setup.
Common questions
What tolerance can you hold when you cut metal on a CNC machine?
On our five-axis and mill-turn centers we hold ±0.005 mm (±0.0002 in) on critical features, with reports on request. That figure assumes a stable setup and a material that does not move after cutting.
Thin walls, long unsupported sections, and stress-relieved or annealed stock can shift after the part comes off the table. If a dimension is critical, say so on the drawing so we can plan the operation order around it.
Which metals can you machine?
Aluminum 6061, 7075, 2024, 5052 and 6082; stainless 303, 304, 316L, 17-4PH and 440C; steel 1018, 1045, 4130, 4140 and 4340; copper and brass alloys; titanium TA2 and TC4; Inconel; magnesium; and engineering plastics including POM, PEEK and PC.
Each group needs its own tool, coating, and cutting data. Sending the same program to 6061 and to Ti-6Al-4V is how tools break.
Do you need a minimum order quantity?
No. We run from a single prototype to 10,000+ part runs. The setup cost is spread over the batch, so the price per part drops as the quantity rises.
For first articles we usually cut one part, measure it, and adjust before running the rest.
How fast can you quote and ship?
Quotation and free DFM analysis come back within 12 hours. Production can start within 24 hours, and parts typically ship in 3–5 days.
Our historical late-delivery probability is below 2%. If a date is tight, tell us at quoting and we will confirm what the schedule allows.
Can you work from a STEP file and a drawing?
Yes. Send the 3D model plus a drawing with tolerances, material, finish, and any critical features marked. If there is no drawing, we machine to the model with a general tolerance and flag anything that looks tight.
Uploads are secure and confidential. An NDA is available on request.
What surface finishes are available?
As-machined finishes run Ra 1.6–3.2 μm, with Ra 0.8–1.6 μm or Ra 0.2–0.8 μm on request. We also offer anodizing, electroless nickel, zinc, silver and gold plating, powder coating, black oxide, bead blasting, tumbling, brushing and polishing.
Laser marking and engraving are available with a minimum character height of 1.5 mm.
Send us the part you need cut
Upload your model and drawing. You get a quote and a free DFM analysis within 12 hours, with no minimum order quantity.
12-hour quote100% inspectionNo MOQNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
