CNC Metal Cutting Basic Guide
This CNC metal cutting basic guide explains what happens where the tool meets the metal, how the machine turns a CAD model into a finished part, and where the process stops making sense. Written for design engineers and buyers who need to judge a part before they send it out.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
How a CNC metal cutting operation actually removes material
Every CNC metal cutting operation is a controlled fracture. A tool edge, harder than the workpiece, is pushed into metal until the material ahead of it shears away as a chip. Nothing melts and nothing is burned away. If the edge is sharp and the feed per tooth is deep enough, the chip forms cleanly and most of the heat leaves with it.
A 3-axis mill moves the tool along X, Y and Z while the spindle turns. A lathe does the opposite: the part rotates and a single-point tool travels along its length. Both read the same kind of instruction. CAM software slices the CAD model into toolpaths, then posts them as G-code with feed rate, spindle speed, depth of cut and coolant commands.
The cut is never perfectly rigid. Tool, holder, spindle and workpiece all deflect a little under load. That deflection is why a light finishing pass exists. Roughing at 1–3 mm depth of cut clears volume fast, then a 0.2–0.5 mm finishing pass brings the wall back to size and holds ±0.005 mm on a stable setup.
Chip evacuation matters as much as the cut itself. A chip that stays in the pocket gets recut, heats the edge and pushes the tool off line. Air blast, through-spindle coolant or a high-pressure flood all solve the same problem: get the chip out of the way before the next tooth arrives.
What each metal does where the tool meets the metal
Aluminum 6061 and 7075 cut fast and throw a long stringy chip. Use 2 or 3 flute end mills with a high helix, 300–600 m/min surface speed, and a water-soluble flood coolant to stop built-up edge. 7075 is stronger but more abrasive on the edge, so keep the radial engagement light on deep pockets.
Stainless 304 and 316 work-harden. If the tool rubs instead of cutting, the surface gets harder and the next pass is worse. Take a heavier feed per tooth, never dwell in the cut, and use plenty of coolant. 17-4PH in the H900 condition is tougher still; rough it as close to final as you can before heat treat.
Carbon steel 1018 and 1045 behave well with coated carbide at 150–250 m/min. 4140 and 4340 need lower surface speed and a rigid setup, because the material pulls the tool into the cut. Titanium TC4 and Inconel 718 are different again: low speed, high feed, flood coolant, and a fresh edge on every job, or the tool will fail mid-pass.
Fixture, workholding and how many setups a part needs
Every setup adds a new datum and a new source of error. A part machined in five setups carries five stack-ups. A 5-axis center or a mill-turn center can often finish the same geometry in one or two. That is the main reason to move a part to a 5-axis machine: not speed, but the removal of re-fixturing.
Soft jaws bored to the part profile hold round and thin-walled parts far better than a standard vise. For a wall under 2 mm, support the back with a potting compound or a sacrificial backing plate, then take light finishing passes of 0.1–0.2 mm. The part will move when the material is removed, and no fixture can prevent that entirely.
Thin plates and long shafts are the classic deflection cases. A 4,000 mm shaft overhangs and whips; support it with a steady rest or turn it between centers with a follow rest. A thin plate bows when clamped, so clamp lightly, face one side, flip, and face the other before drilling anything through.
Probing in the machine sets the work offset from the actual stock rather than from a drawing. On castings and forgings with 1–2 mm stock variation, that step decides whether the part cleans up on all faces or ends up undersize on one.
Tolerance, surface finish and what the machine can hold
Tolerance and finish are two separate promises. A dimension can hold ±0.005 mm while the surface is still Ra 3.2 μm. Or the surface can be Ra 0.2 μm on a part that is 0.05 mm out of position. Decide which one the function actually needs before you put both numbers on the drawing.
Roughly, turning holds tighter diameter tolerance than milling because the tool stays in continuous contact. Bores and reamed holes hold position well; deep pockets in a corner do not. A tight tolerance on a free-standing wall or a thin floor is the most common drawing mistake we see.
Surface finish follows the tool and the stepover. A Ra 0.8–1.6 μm finish is a normal machined result. Ra 0.2–0.8 μm needs a finishing tool, a small stepover and a stable setup. As-machined Ra 1.6–3.2 μm is fine for brackets, housings and anything that gets painted or powder coated.
Add a tolerance only where it is needed. Over-tolerancing drives extra setups, extra inspection and a slower cycle, and it rarely improves how the part works.
Where CNC metal cutting stops being the right call
CNC cutting wins on complex geometry, tight tolerance and low to medium volume. It loses on thin, uniform, high-volume parts. A stamped bracket at 100,000 pieces per year costs a fraction of the machined version. A die-cast housing with 1 mm walls is cheaper per part than a machined one, and the tool that makes it lasts for years.
Very hard material is another boundary. Above roughly 45 HRC, cutting gets slow, tool life drops and the cost per part climbs fast. If the part must be that hard, machine it soft, heat treat, then grind or EDM the critical features. Hard milling exists, but it is a specialty process, not a general answer.
Feature size sets the other limit. A slot 0.5 mm wide and 10 mm deep is a tool-breakage job. The rule of thumb for end mills is depth no more than 3× diameter in aluminum and 1.5× diameter in steel, unless you use a reduced-neck tool and accept the risk. Very small internal radii force a small tool, and a small tool forces light passes.
If the geometry is mostly flat, uniform and repeated, ask whether sheet metal, casting or molding fits better. Machining is the right answer when the part is complex, low volume, or needs to be finished and shipped in days.
Material and feature: what to expect from each cut
Typical shop-floor ranges on a rigid setup. Use them as a starting point, not a guarantee.
| Workpiece | Surface speed | Main risk | Practical note |
|---|---|---|---|
| Aluminum 6061 / 7075 | 300–600 m/min | Built-up edge | High-helix tool, flood coolant |
| Stainless 304 / 316 | 80–150 m/min | Work hardening | Heavy feed, no dwell in cut |
| Steel 1018 / 1045 | 150–250 m/min | Chip packing | Coated carbide, air or flood |
| Steel 4140 / 4340 | 100–180 m/min | Tool pull-in | Rigid setup, lower speed |
| Ti-6Al-4V (TC4) | 40–80 m/min | Heat at the edge | Fresh edge, high feed, flood |
| Inconel 718 | 25–50 m/min | Notch wear | Low speed, constant coolant |
| Thin wall under 2 mm | Reduce 30–50% | Deflection | Light passes, back support |
One decision rule
For complex geometry, tight tolerance and runs from one piece to a few thousand, cut it from solid on a CNC. For thin walls, uniform sections and high annual volume, move the part to stamping, casting or molding and machine only the critical faces.
Common questions
Does coolant always improve the cut?
Not always. In aluminum and steel, flood coolant clears chips and controls heat, so it helps. In cast iron, dry cutting with air blast often works better because the graphite in the chip lubricates the edge and coolant turns the dust into a sludge that packs the flutes.
In titanium and Inconel, high-pressure coolant is close to mandatory. It breaks the chip and keeps heat out of the edge. If you cannot supply high pressure, lower the speed and accept a longer cycle.
Why does my part measure correctly on the machine but fail inspection?
The usual causes are temperature and clamping. A part cut warm shrinks as it cools, so a bore measured at 30 °C can be undersize at 20 °C. Aluminum moves about 23 μm per meter per degree Celsius, which is enough to matter on a 200 mm bore.
The second cause is release. A thin part clamped during cutting springs back when the vise opens. Measure it free, on a granite plate, after it reaches room temperature.
How deep can a pocket be cut?
With a standard end mill, keep depth under about 3× tool diameter in aluminum and 1.5× in steel. Beyond that, the tool deflects, the wall bell-mouths and the finish gets worse toward the bottom.
A reduced-neck or long-reach tool extends the range, but it flexes more, so reduce feed and depth per pass. Deep pockets are also where chip evacuation fails first. If chips recut, the tool will break.
Is 5-axis always better than 3-axis?
No. A flat plate with holes on one face is faster and cheaper on a 3-axis machine. Five-axis pays off when the part has features on several faces, curved surfaces, or undercuts that would need multiple fixtures.
It also helps when a single datum matters. Cutting five faces in one setup removes the re-fixturing error, which is often worth more than the higher hourly rate.
What file do you need for a quote?
A STEP or IGES model plus a 2D drawing with tolerances, material and finish. The model defines geometry; the drawing defines the acceptance criteria. If there is no drawing, state the critical dimensions in writing.
We return a quotation and a DFM analysis within 12 hours. Production can start within 24 hours after the drawing is frozen.
How is confidentiality handled?
Uploads are secure and confidential. We can sign an NDA before you send the model, and we do not show customer parts or drawings in public material without written permission.
If your part is under NDA, tell us at the quote stage so the files stay inside the restricted project folder.
Send a part and get a machining plan
Upload your model and drawing. We come back with a quotation and a DFM analysis within 12 hours, then cut the part on the machine that fits it.
12-hour quote100% inspectionNo minimum order quantity
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
