CNC milling explained: what the spindle actually does

• 1
  How the cut happens: spindle, feed, and chip load
• 2
  3-axis, 4-axis, and 5-axis: what each one buys you
• 3
  Tool reach, corner radii, and wall stiffness
• 4
  What ±0.005 mm and Ra 0.8 μm really require
• 5
  How material choice changes the cut
• 6
  Choosing the process by part geometry

CNC milling is subtractive. A blank is clamped to a table or a vise, and a multi-flute cutter spins while the machine moves it along programmed paths. The controller reads G-code generated from CAD/CAM, then drives ball screws and linear guides to position the tool. Nothing is formed or cast. Material leaves the block as chips.

Three numbers decide whether that cut is stable: cutting speed, feed per tooth, and radial depth of cut. Feed per tooth is the chip thickness each flute takes. Push it too high and the tool edge chips. Drop it too low and the edge rubs instead of cutting, which work-hardens stainless and burns the coating off the tool. On 6061 aluminium we typically run 300–600 m/min surface speed and 0.05–0.15 mm per tooth on a Ø10 mm three-flute end mill.

Chip evacuation matters as much as the numbers. A deep pocket with no coolant path recuts chips, raises temperature, and ruins both finish and tool life. Through-spindle coolant, air blast, or a high-pressure nozzle solves most of it. On titanium and Inconel we slow down and flood the cut, because those alloys carry heat into the tool rather than the chip.

• 1
  Rubbing beats chippingToo light a feed dulls the edge faster than a proper chip load.
• 2
  Heat follows the chipIn aluminium most heat leaves with the chip; in titanium it stays in the tool.
• 3
  Clear the pocketIf chips cannot exit, no speed or feed setting will save the finish.

A 3-axis mill moves X, Y and Z. The tool always approaches from one direction, so every face you need to machine has to be reachable from the top or reached by re-fixturing the part. This is fine for plates, brackets, housings with open pockets, and most parts under 500 mm. It is the cheapest and fastest route when the geometry allows it.

A 4-axis mill adds rotation around one axis, usually A. The part turns while the tool cuts, so you can machine around a cylindrical body in one setup. Think shafts with milled flats, cam profiles, and parts with features on multiple sides of a round blank. Setup count drops, and so does the stack-up of positioning errors between setups.

5-axis adds a second rotary axis, tilting either the tool or the table. The cutter can stay normal to a curved surface, which is what makes impellers, turbine blades, and deep cavities with undercuts practical. The real gain is not exotic shapes. It is fewer setups, shorter tools, and better reach into pockets that a 3-axis machine would need a long, chatter-prone tool to touch.

• 1
  3-axisPrismatic parts, one dominant access direction.
• 2
  4-axisRound or rotating parts with features on several sides.
• 3
  5-axisCurved surfaces, undercuts, and parts that need one setup.

Every internal corner carries the radius of the cutter that made it. A Ø6 mm end mill cannot leave a sharper than 3 mm inside radius. If your drawing calls for a sharp internal corner, someone has to broach it, EDM it, or you accept a radius. Deciding this at the design stage saves a quote revision later.

Depth-to-diameter ratio sets how much the tool deflects. Past about 4:1, a standard carbide end mill starts to chatter and the wall finish goes cloudy. Long-reach tools, reduced neck shanks, or a 5-axis approach that keeps the tool short all help. If a pocket is 80 mm deep and 20 mm wide, you are at 4:1 before you even pick a tool.

Thin walls move. A 1 mm wall on a 100 mm aluminium part will deflect under clamping pressure and again under cutting force. Rough it leaving 0.3–0.5 mm of stock, let it cool, then finish with light passes. For walls under 1 mm, expect to add a support rib or accept a looser tolerance. This is a stiffness problem, not a machine problem.

• 1
  Corner radiusMatches the smallest cutter you are willing to pay for.
• 2
  Reach ratioKeep depth under about 4× diameter where you can.
• 3
  Wall thicknessBelow 1 mm, plan on support or relaxed tolerance.

Tolerance and surface finish are two separate costs. Holding ±0.005 mm on a feature needs a controlled shop, temperature-stable measurement, and a process that was proven on that geometry. It does not mean the whole part is held to ±0.005 mm. Put the tight tolerance only on the features that need it, usually a bore, a mating face, or a datum.

Surface finish follows tool path and feed. As-machined at Ra 1.6–3.2 μm is what a normal finishing pass leaves. Ra 0.8–1.6 μm needs a finer stepover and a sharp tool. Ra 0.2–0.8 μm usually means a dedicated finishing pass, sometimes with a smaller tool, and it takes longer. Bead blasting, tumbling, or polishing can hit a cosmetic spec without the machining time.

Measurement is part of the spec. If you need a report on a bore diameter, say so up front. We inspect 100% of parts before shipment, covering raw material check, in-process monitoring, and final inspection, and reports are available on request. Parts that need CMM data on every unit should be flagged at quote time, not after.

• 1
  Tight where it mattersApply ±0.005 mm only to functional features.
• 2
  Finish has a cost curveEach step finer in Ra adds machining time.
• 3
  Say what you measureNamed dimensions in the RFQ avoid disputes later.

Aluminium 6061 and 7075 cut fast and hold a good finish. 7075 is stronger but more prone to stress movement after heavy stock removal, so rough and finish in separate operations on tight parts. Stainless 303 machines cleanly; 304 and 316L work-harden if the tool rubs, so keep the feed up and never dwell in the cut. 17-4PH in the H900 condition is harder on tooling and needs slower speeds.

Titanium Ti-6Al-4V and Inconel are the slow end. They conduct heat poorly, so the cutting edge runs hot, and they spring back under load. Expect lower speeds, more coolant, and more frequent tool changes. Inconel is normally the last resort for a milled feature. If the part can be made in another alloy or cast, that is usually the better call.

Plastics behave differently again. POM and ABS cut easily but melt if the feed is too slow. PEEK is abrasive and expensive, so leave enough stock for a clean finishing pass. Carbon fibre eats tool edges, so plan on coated tooling and a shorter tool life. The right answer for each material is a speed and feed combination proven on that alloy, not a generic chart.

• 1
  AluminiumFast, forgiving, good finish. Watch stress movement in 7075.
• 2
  Stainless and titaniumKeep the feed up, control heat, expect tool wear.
• 3
  PlasticsAvoid melting; PEEK and carbon fibre raise tooling cost.