CNC Milling Guide: How the Cut Actually Works
A working CNC milling guide for design and sourcing engineers who need to know what a milling cutter can and cannot do. It covers chip formation, axis count, tolerance and wall-thickness limits, and the cases where milling is the wrong process. Read it and you can judge a part before you send it for quote.
Key takeaways
What happens at the cut
Milling is a chip-removal process. A spindle turns a multi-edge cutter, the machine moves that cutter along controlled axes, and each edge shears a chip off the workpiece. Nothing is formed or cast. The final geometry is whatever the tool path leaves behind.
That single fact explains most design rules. Every feature has to be reachable by a rotating cylinder of a known diameter. A cutter is rigid in the radial direction and weak in the axial direction, so it cuts walls well and floors less well as it gets longer.
Heat and force both scale with the chip you are trying to take. Hard materials and deep cuts push cutting force up, which pushes tool deflection up, which shows up on the part as taper, chatter marks or a wall that is thinner at the bottom than the top.
- 1Chip loadMillimeters of material removed per tooth per revolution; too small rubs, too large breaks edges.
- 2Radial engagementHow much of the cutter diameter is buried in the material at once.
- 3Axial depthHow far the cutter reaches down; the main driver of deflection on long tools.
How axis count changes the plan
A three-axis mill moves the tool in X, Y and Z only. The part sits still. To machine a second face you unclamp it, rotate it, and clamp it again. Every re-clamp adds a small positioning error, and on a part with five faces that error can stack past your tolerance band.
A four-axis mill adds rotation about one axis, usually a rotary table like a Ø400 mm table. This suits parts that are mostly cylindrical with flats and slots around the circumference, such as shafts with milled keyways or cam profiles.
Five-axis machines add two rotary axes. The tool can approach the workpiece from nearly any direction, so undercuts, angled faces and deep pockets on different planes come off in one setup. The accuracy benefit is not the machine itself, it is the setups you no longer perform.
- 1Three-axisFlat plates, pockets, slots, one dominant direction of access.
- 2Four-axisRotational parts with milled features, drilled hole patterns around a diameter.
- 3Five-axisComplex contours, five-sided parts, tight true-position callouts across faces.
Tolerance, wall thickness and surface finish
Tolerance and surface finish are bought separately. A part can hold ±0.005 mm on a bore and still have a rough as-machined face somewhere else. When you call out a tight tolerance, say which surfaces need it. A blanket tolerance note on the whole drawing raises cost with no functional gain.
Wall thickness is the quiet killer. A 0.5 mm wall in aluminium is machinable but sings during the final pass. A 0.5 mm wall in stainless needs light radial cuts and sharp tooling, and even then the floor may bow. Below roughly 0.8 mm, expect to discuss support, fixturing and possibly a redesign.
Surface finish on milled faces comes from the tool path, not from a magic setting. A fine stepover and a sharp cutter get you to Ra 0.8–1.6 μm on most metals. Going below that usually means a separate finishing operation, and Ra 0.2–0.8 μm is reserved for faces that truly need it.
- 1As-machinedRa 1.6–3.2 μm, standard cutter path, no extra operation.
- 2Fine milledRa 0.8–1.6 μm, tighter stepover, slower feed on the finish pass.
- 3Polished or lappedRa 0.2–0.8 μm, separate process, added cost and handling risk.
Why the same geometry behaves differently in 6061 and 316
Aluminium 6061 cuts fast and leaves a clean face. It also moves when you release the clamp, because the residual stress from the plate is now free to bend the part. If a thin aluminium plate has a flatness callout, expect the shop to rough it, let it relax, then finish it.
Stainless 316 work-hardens. If the cutter rubs instead of cutting, the surface gets harder and the next pass is worse. That is why a stainless part with a deep narrow slot often costs more than the same slot in aluminium, even though the geometry is identical.
Titanium Ti-6Al-4V and Inconel push heat into the tool rather than the chip. Tool life drops, feed rates drop, and the shop may prefer a five-axis setup so it can keep the cutter engaged at a constant load instead of stopping and starting.
- 1Aluminium 6061, 7075Fast, good finish, watch residual stress on thin plates.
- 2Stainless 303, 304, 316303 is free-cutting; 316 work-hardens and needs constant feed.
- 3Titanium and InconelSlow, hot, expensive to cut; design for fewer operations.
- 4Plastics POM, PEEKClamp lightly, use sharp tools, coolant choice matters.
Axis count against real part features
Pick the lowest axis count that still holds the tolerance.
| Feature | Three-axis | Four-axis | Five-axis |
|---|---|---|---|
| Flat plate with pockets | One setup, fast | Overkill | Overkill |
| Shaft with milled flats | Two or three setups | One setup | One setup |
| Angled face at 35° | Needs an angle plate | Limited reach | One setup, tool tilts |
| Five-sided housing | Four or more setups | Not practical | One setup |
| Deep undercut pocket | Cannot reach | Cannot reach | Reachable with stub tool |
| Hole pattern on a cone | Hard to fixture | Partial | One setup |
| ±0.005 mm across faces | Stacked setup error | Risky | Best chance |
| One-off prototype bracket | Cheapest path | Sometimes | Only if geometry needs it |
When to mill and when not to
If the part is a solid block with pockets, flats and moderate walls, mill it and keep the design to three axes. If true position across several faces is tight, or the geometry has undercuts and angled faces, pay for five-axis and remove the setups. If the part is a thin shell with a deep small hole or a sharp internal corner, change the design or change the process.
Common questions about CNC milling
What is the smallest internal corner radius I can specify?
The corner radius equals the cutter radius. A 6 mm cutter leaves a 3 mm corner. If you need a smaller corner, the shop has to use a smaller cutter, which is shorter and less rigid.
On deep pockets, a small corner radius and a deep floor together are the expensive combination. Add a relief or open the corner where the function allows it.
How deep can a pocket be before cost climbs?
A common working limit is about four times the cutter diameter in depth for a rigid setup. Past that, the tool sticks out too far and you lose accuracy and finish.
If the pocket is deeper than that, expect a larger corner radius, a rougher floor, or a redesign that splits the feature into two shallower steps.
Do I need to add chamfers and fillets on my drawing?
Yes, and they help the shop. A chamfer on a sharp edge removes a burr that would otherwise need hand work, and a fillet at an inside corner spreads load and lets a larger cutter pass.
Undimensioned sharp edges usually get a small break edge by hand, which is fine for function but not repeatable across a 10,000 part run.
When does a hole belong on a mill and when on a lathe?
Centered holes in a rotational part belong on a lathe, where the part turns and the tool stays still. Off-axis holes, holes on a flat face, and hole patterns in a plate belong on a mill.
If a part has both, a mill-turn center does both in one setup, which protects the relationship between the bore and the milled features.
Why does my part measure right on the machine but wrong after shipping?
Usually it released stress. The material was clamped flat, the cut removed material from one side, and the balance of internal stress changed. Once the clamps come off, the part moves.
The fix is process, not inspection: rough, stress-relieve or rest, then finish. Talk to the shop before you tighten the flatness callout.
Can milling hold ±0.005 mm on every dimension?
No, and no shop should say yes. ±0.005 mm is achievable on specific features with the right machine, fixturing and temperature control.
A drawing that calls it on every dimension forces the shop to inspect everything at that level. Mark the critical dimensions and let the rest sit at a general tolerance.
Send the drawing, get a real answer
Upload your model and we return a quotation plus a DFM analysis within 12 hours. We flag the features that will drive cost before you commit to a tool.
12-hour quote100% inspectionNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
