CNC process explainer

CNC Milling Basics and Uses

A shop-floor explanation of how a rotating cutter removes metal, why axis count changes what you can hold, and which parts belong on a mill instead of a lathe. Written for engineers and buyers who need to read a drawing and pick a process.

Get Instant Quote Talk to an Engineer

±0.005 mmRa 0.2–0.8 μm5-axis and 3-axis1 pc to 10,000+

High-precision CNC milling basics and uses

On this page

How a CNC mill removes material

A CNC mill holds the workpiece in a vise, fixture or chuck and spins a multi-tooth cutter in a spindle. The table moves the part under the tool, or the spindle moves over it, following coordinates that come from CAM software. Every pass is a set of positions and feed rates, not a machinist turning handwheels.

Cutting happens at the tip of each flute. A two-flute end mill in aluminium 6061 might run 8,000 rpm with a 2,000 mm/min feed; the same cutter in 316 stainless drops to roughly 1,500–2,500 rpm and a fraction of that feed. Too much speed burns the edge, too little rubs and work-hardens the surface.

Three numbers decide the result: cutting speed (surface meters per minute), feed per tooth, and axial depth of cut. Get them wrong and you hear it before you measure it. Chatter, a bright ringing noise, means the setup is flexing or the cutter is overhung.

Roughing removes bulk stock in a few heavy passes. Finishing follows with light passes, often 0.1–0.3 mm radial engagement, to reach Ra 0.8–1.6 μm. Separating the two operations is cheaper than chasing a fine finish with a worn roughing tool.

1
Climb millingTooth enters at full chip thickness. Default on modern machines with ball screws.
2
Conventional millingRarely used now; leaves a work-hardened skin on stainless.
3
CoolantFlood for steel and titanium, air blast or mist for aluminium and plastics.

Axis count

3-axis vs 4-axis vs 5-axis: what changes on the drawing

A 3-axis mill moves X, Y and Z. The tool always points down. Any feature on a side face needs a second setup, which means a second fixture, a second datum and a fresh stack of tolerance. For flat plates and simple pockets that is fine and cheap.

A 4-axis machine adds a rotary table, usually the A-axis about X. Cylindrical work, slots around a shaft and features on four sides of a block can run in one setup. Our rotary tables are Ø400 mm, which suits most shaft and manifold work.

A 5-axis machine adds a second rotary axis, so the tool can tilt. Undercuts, deep angled holes, impeller blades and free-form surfaces get cut without repositioning. That matters most where the datum is the hard part. One setup means one tolerance stack instead of four.

Five axes is not automatically better. Rigidity drops as axes stack up, and programming time rises. A flat bracket with three holes is faster and cheaper on a 3-axis machine. Reach for 5-axis when the geometry is genuinely 3D or when repositioning would break a tight tolerance.

1
Choose 3-axisPrismatic parts, flat faces, through holes, open pockets.
2
Choose 4-axisShafts, bushings, parts with features on four sides.
3
Choose 5-axisUndercuts, contoured surfaces, tight position between angled features.

Boundaries

Where milling stops working well

Deep, narrow pockets are the classic limit. A cutter needs to reach the bottom without rubbing its shank on the wall. Past about 4× diameter in depth, a long tool deflects and the wall tapers. If a pocket is 10 mm wide and 80 mm deep, expect to drill, wire-cut or rethink the design.

Sharp internal corners are another. A rotating cutter leaves the radius of its own diameter. A 6 mm end mill leaves roughly a 3 mm corner radius. If the print calls for a sharp inside corner, the part needs EDM, broaching or a design change to add a relief.

Thin walls move. Aluminium below 1 mm wall thickness, or steel below 1.5 mm, will deflect under clamping and cutting pressure. Bring the wall up, add a temporary rib, or plan a stress-relief step between roughing and finishing.

Hardened material above roughly 45 HRC is usually ground or EDM work. Milling it needs carbide or ceramic tooling, light passes and a rigid setup. It is possible, but the cost per part climbs fast.

1
Depth-to-diameterKeep under 4× for end mills without special holders.
2
Corner radiusSmaller cutter, smaller radius, but slower material removal.
3
HardnessAbove 45 HRC, compare milling cost against grinding before committing.

Materials

Material behavior on the mill

Aluminium 6061 and 7075 cut fast and hold a good finish. 6061 is the general-purpose choice; 7075 gives higher strength but machines with a sharper edge and less tolerance for dwell. Both can reach Ra 0.8 μm with a clean finishing pass.

Stainless 304 and 316 work-harden if the cutter rubs. Keep the feed per tooth up and never let the tool dwell in the cut. 17-4PH in the solution-treated condition mills reasonably and then ages to high strength, which is why it shows up in aerospace and medical parts.

Titanium Ti-6Al-4V and Inconel generate heat at the cutting edge and conduct it poorly. Speeds drop hard, coolant flow has to be heavy, and tool life is measured in minutes rather than hours. Budget for more passes and more inspection.

Plastics behave differently. POM and PEEK cut cleanly with sharp, polished flutes and high spindle speed; ABS and PC soften and gum if the feed is too slow. Climb milling with an air blast usually beats flood coolant here.

1
Aluminium6061, 7075, 2024, 5083, 6082, ADC12.
2
Stainless303, 304, 316L, 17-4PH (SUS630), 440C.
3
Titanium and nickelTA1, TA2, TC4 (Ti-6Al-4V), Inconel.
4
PlasticsABS, PC, POM, PA, PEEK, PP, carbon fibre.

Measurement

Holding tolerance and proving it

A tolerance callout only means something if the shop can measure it. ±0.005 mm on a bore needs a controlled temperature and a good micrometer or CMM, not a caliper on the bench. On long parts, thermal drift moves the number while you measure.

In-process checking catches trouble before the run is finished. We check raw material certificates on arrival, monitor critical dimensions during cutting, and inspect 100% of parts before shipment. Reports go out on request with the dimensional data.

Surface finish and tolerance interact. A tight bore with a rough wall will not seal or fit properly. If a drawing asks for both ±0.01 mm and Ra 0.4 μm, plan a separate finishing pass with a fresh tool and a light radial engagement.

First-article inspection is the cheapest insurance on a new design. One part measured fully before the run starts finds the datum error, the missing chamfer or the wrong thread callout while it is still a programming fix.

1
Calipers±0.02 mm at best. Not for final acceptance.
2
Micrometer and bore gaugeFor diameters and holes at ±0.005 mm.
3
CMMFor position, profile and first-article reports.

Selection table

Matching part features to the right milling setup

Read across a row to see what each feature needs and what to watch for.

Part feature	Best setup	Typical tolerance	Watch for
Flat plate with through holes	3-axis, one vise setup	±0.05 mm	Thin plate lift during drilling
Housing with pockets on 5 faces	4-axis or 5-axis	±0.02 mm	Datum shift between setups
Impeller or turbine blade	5-axis simultaneous	±0.01 mm	Tool reach and shank collision
Shaft with cross holes	4-axis with rotary table	±0.02 mm	Rotary table runout
Deep narrow slot, 6 mm wide	EDM, not milling	±0.01 mm	Tool deflection past 4× depth
Hardened die insert, 58 HRC	Grinding or EDM	±0.005 mm	Milling cost climbs sharply
Large frame, 3,000 mm long	3-axis with 4,000 mm travel	±0.05 mm	Thermal growth over long cuts

When to mill, when to look elsewhere

Mill it when the part is prismatic or contoured and needs tight position between features. Switch to turning for round parts with a single axis of symmetry, and switch to EDM or grinding when the feature is a sharp internal corner or the material is above 45 HRC.

Get Instant Quote Talk to an Engineer

FAQs

CNC milling questions engineers ask

What is the difference between CNC milling and CNC turning?

Milling spins the tool and moves the workpiece; turning spins the workpiece and moves a single-point tool. Round parts with one axis of symmetry belong on a lathe. Prismatic parts with pockets, slots and holes on several faces belong on a mill.

Many parts need both. A mill-turn center does the turning and the cross-drilling in one setup, which removes a datum shift and one tolerance stack.

How tight a tolerance can milling actually hold?

On a rigid setup in aluminium or steel, ±0.005 mm is achievable on critical features with in-process checks. Position tolerance across a part depends more on the number of setups than on the machine.

One setup holds tighter than three. If a drawing needs ±0.01 mm between features on opposite faces, plan the process around a single 5-axis setup or expect to pay for the extra inspection.

Which parts are a bad fit for milling?

Very deep narrow slots, sharp internal corners, thin flexible walls and hardened material above 45 HRC. Each has a better process: EDM for corners and deep slots, grinding for hard surfaces, and design changes or temporary ribs for thin walls.

Large flat panels with no 3D features are usually cheaper as sheet metal than as milled plate, because the mill removes material you never needed.

Does axis count change the price much?

Programming and setup time rise with axis count, and machine hourly rates are higher. On a simple bracket, 3-axis wins. On a part with features on five faces, 5-axis often costs less overall because it removes three setups and the errors that come with them.

The honest answer is that it depends on geometry. Send the drawing and the quote will show which route is cheaper.

How do I prepare a drawing for a milling quote?

Give a 3D model plus a 2D drawing that shows datums, critical tolerances, thread callouts, surface finish where it matters, and material condition. Mark which dimensions are functional and which are reference.

Note any features that must stay sharp, any sealing surfaces, and the quantity you expect. That information is what turns a rough price into a real one.