CNC processing work: how material removal actually behaves

• 1
  What happens where the tool meets the metal
• 2
  What tolerance CNC processing work can hold
• 3
  Which parts belong on a mill, a lathe, or neither
• 4
  How material choice changes the cut
• 5
  Choosing the process for your part

CNC processing work is subtractive. A rotating cutter or a turning tool contacts solid stock, and the material in front of the edge shears off as a chip. The machine only controls position and feed. Everything else, heat, force, chip evacuation, is decided by the toolpath and the cutting parameters you set.

The chip carries most of the heat away. When it breaks cleanly and leaves the zone, the part stays cool and the tool lasts. When the chip recrystallizes on the edge, a built-up edge forms, and the surface starts to tear. That is why feed per tooth matters more than spindle speed on most aluminum jobs.

Two numbers describe the cut: surface speed and chip load. Surface speed is how fast the material passes the edge, measured in m/min. Chip load is the thickness of material each tooth takes, usually 0.05–0.15 mm per tooth in aluminum and 0.03–0.10 mm in steel. Push chip load too low and the edge rubs instead of cutting.

Rubbing is the failure mode that costs the most. The tool dulls, the part heats up, and dimensions drift after the cut. A heavier feed with a shallower radial step keeps the edge engaged and the temperature stable. On 6061-T6 we typically run 3,000–6,000 rpm with a 12 mm carbide end mill at 1,500–3,000 mm/min.

Rigidity sets the ceiling on all of this. A small part in a vise on a 3-axis machine behaves differently from the same part on a 5-axis trunnion, because tool overhang and workholding stiffness change the vibration budget. Short tools, short holders, and a supported workpiece do more for accuracy than a faster spindle.

A general machining tolerance of ±0.1 mm covers most brackets, housings, and covers. The number only becomes interesting when you go below ±0.05 mm, because that is where fixturing, thermal drift, and tool wear start to matter as much as the machine's own positioning accuracy.

On our equipment we hold ±0.005 mm (±0.0002 in) on critical features, with a 100% inspection pass before shipment. That figure applies to features measured in a temperature-stable room with a calibrated instrument. It does not mean every dimension on the drawing lands there for free; it means the process can reach it when the feature is designed to be reachable.

Reachability is the part most drawings ignore. A bore with a depth-to-diameter ratio above 4:1 needs a boring bar or a long-reach tool, and deflection grows with the square of overhang. A tight tolerance on a deep, small-diameter feature is a different job from the same tolerance on a flat face.

Datums matter just as much. If the drawing stacks five tolerances off one corner, the machinist has to hit every one of them at once. Distribute tolerances across functional datums and the same part gets cheaper without losing function.

Surface finish follows a similar logic. As-machined surfaces land at Ra 1.6–3.2 μm. Finer cuts, smaller stepovers, and a finishing pass bring that to Ra 0.8–1.6 μm, and polishing or lapping can reach Ra 0.2–0.8 μm when the geometry allows access.

Milling removes material with a rotating multi-tooth cutter while the work stays still or indexes. It suits pockets, slots, faces, and prismatic shapes. Turning spins the work against a single-point tool, which suits shafts, bushings, and any part whose main feature is a surface of revolution.

Mill-turn centers combine both in one setup. On a part like a hydraulic manifold with a turned spigot and a milled port face, doing both operations without re-clamping removes one datum shift and one queue. We run 16 mill-turn centers for exactly that reason.

5-axis work earns its cost when the part has features on several faces, deep cavities, or a contoured surface that would need many setups otherwise. We run 16 simultaneous 5-axis machining centers. On a part with features on four sides, one 5-axis setup usually beats four 3-axis setups on both accuracy and total time.

Some geometry still does not belong on a mill. Thin walls below 0.5 mm deflect under cutting force. Deep narrow slots below 2 mm wide need tools that cannot clear chips. Sharp internal corners cannot be cut by a round tool; the corner radius equals the tool radius unless you specify EDM.

Cost follows setup count more than cycle time on low volumes. A part that fits in one 5-axis setup with no custom fixture is often cheaper at 50 pieces than a simpler part that needs three fixtures and two operations.

There is also a size ceiling. Our largest travel is 4,000 × 400 × 150 mm, with medium envelopes at 750 × 1,150 × 550 mm and 600 × 600 × 600 mm. Beyond that, the part gets split or moves to another process.

Aluminum 6061-T6 is the default for prototypes and functional parts. It cuts fast, holds a good finish, and anodizes cleanly. 7075 gives higher strength but machines with more spring and is harder to anodize evenly. 2024 sits between them and is common in aerospace brackets.

Stainless 304 and 316 work-harden. The first pass has to cut under the hardened layer, not rub on it. That means a heavier feed and a sharp, coated tool. 17-4PH in the H900 condition is harder again but holds dimensions well after heat treat, which matters for shafts and valve parts.

Steel grades 1018 and 1045 machine predictably. 4140 and 4340 need lower surface speeds and more attention to heat. Titanium TC4 (Ti-6Al-4V) cuts at roughly one third the speed of aluminum and conducts heat poorly, so the tool takes the temperature. Coolant delivery matters more than rpm.

Plastics behave differently again. POM and PA cut cleanly with sharp tools and high rake. PEEK needs higher temperatures at the edge to avoid chipping. Carbon fibre composites wear tools fast; we count edges rather than hours on those jobs.

Material also sets what happens after machining. Hardcoat anodizing adds 0.025–0.05 mm per surface and changes the fit on a tight bore. Electroless nickel adds a more even layer. Plan the finish before you fix the tolerance, or the coating will eat your clearance.