CNC machining: how the cut actually happens

• 1
  What actually happens at the cutting edge
• 2
  Where ±0.005 mm comes from and where it does not apply
• 3
  Which features push a part to 5-axis
• 4
  Material behavior changes the plan more than the machine
• 5
  When CNC machining is the wrong answer
• 6
  Feature and volume: which process fits

CNC machining removes material with a rotating cutter that is driven along a programmed path. The tool does not scrape the surface. It shears a chip off the workpiece, and the chip carries most of the heat away with it. Everything else on this page follows from that one fact.

The shear happens in a zone a few hundredths of a millimeter wide. Rake angle, edge radius, cutting speed and feed per tooth set how much deformation the material sees before it separates. Aluminium 6061 shears cleanly at 300–600 m/min with sharp carbide. Ti-6Al-4V does not, because its low thermal conductivity keeps heat in the edge, so surface speed drops to 40–80 m/min and the tool wears faster.

Rigidity matters as much as the tool. A cutter hanging 80 mm out of a 12 mm holder deflects under load, and that deflection lands directly in the part as wall taper or chatter marks. Shorten the gauge length, increase the shank diameter, or reduce radial engagement. The programming fix is cheaper than the tooling fix, and both are cheaper than re-cutting a scrapped part.

Tolerance is a system property, not a machine property. A five-axis center that holds ±0.005 mm on a 50 mm aluminium bracket will not hold it on a 900 mm steel weldment, because thermal drift and material springback scale with size and with hardness. Treat any quoted number as valid only for the size and material class it was measured on.

On aluminium parts under roughly 300 mm, ±0.005 mm is routine for bored holes, turned diameters and flat mating faces. On stainless 316L or 17-4PH the same callout costs more because the tool wears through the cut and the operator has to compensate mid-run. On thin walls the limit is usually deflection, not the machine.

Surface finish and tolerance are separate budgets. Ra 1.6–3.2 μm is an as-machined finish straight off a sharp cutter. Ra 0.8–1.6 μm normally needs a finishing pass with a smaller stepover or a wiper insert. Ra 0.2–0.8 μm usually means a ground or lapped operation comes after CNC machining.

A drawing that puts a tight tolerance on a non-functional surface only moves cost. Ask which faces locate the part in the assembly. Tighten those. Leave the rest at general tolerance, and mark datum features so the shop can plan the setup order.

A three-axis machine can only reach the part from one direction per setup. Every additional face means another setup, another fixture, and another chance for stack-up error. Five-axis work is not about looking advanced. It is about reaching features without re-clamping.

Angled ports, undercuts, compound curves and deep pockets with non-parallel walls are the usual triggers. Mill-turn centers handle parts that need both a turned diameter and off-axis milled features, because the part is cut in one clamping. That removes the concentricity error you would otherwise get from moving between a lathe and a mill.

The trade-off is access, not accuracy. Five-axis toolpaths are longer, simulation takes more engineering time, and fixtures are often simpler but the setup is slower. On a simple plate with through-holes, a three-axis machine with two setups is faster and cheaper. Push to five axes when the feature count per face is high.

Size sets the ceiling. Our largest travel is 4,000 × 400 × 150 mm on the long-bed machines. Mid-size work runs on 750 × 1,150 × 550 mm and 600 × 600 × 600 mm envelopes, and compact parts use 500 × 500 × 450 mm or 500 × 310 × 200 mm. Rotary work up to Ø400 mm covers most round parts.

Aluminium 6061-T6 and 7075 cut fast and hold tolerance well. They are the default for prototypes, brackets, housings and heat sinks. 7075 is stronger but galls more, so thread milling beats tapping on small threads. 2024 has poor corrosion resistance unless it is anodized or plated.

Stainless 303 machines freely because of its sulfur content, which is why it shows up in shafts and fittings. 304 and 316L are tougher, work-harden quickly, and punish light repeated passes. Feed through the hardened skin instead of rubbing it. 17-4PH in the H900 condition machines closer to a tool steel and needs slower speeds.

Titanium TC4 (Ti-6Al-4V) and Inconel sit at the other end. Both hold heat at the edge, both work-harden, and both consume tooling at a rate that shows up in the price. Design thin titanium webs with generous radii. A sharp internal corner is where cracks start in service.

Plastics behave in the opposite way. POM and PEEK cut cleanly but move with temperature, so tolerance should be checked after the part cools, not on the machine. ABS and PC are prone to melting at the edge if the feed is too slow. Carbon fibre needs diamond tooling, or the edge frays.

CNC machining wins on tight tolerance, on hard materials, and on low to mid volumes where tooling cost would never amortize. It loses on hollow, thin-walled shells in high volume, where injection molding, die casting or vacuum casting produce the same shape in seconds.

It also loses on parts that are mostly empty space. If 70% of the stock has to be removed to reach the geometry, the cycle time is paying for chips. A casting or a fabricated weldment with a few machined interfaces is usually cheaper, provided the tolerance you actually need sits only on those interfaces.

Sheet metal fabrication beats CNC machining for enclosures, brackets and panels under about 3 mm thick. Bending is fast, and the flat pattern is easy to revise. Reach for a machined block only when the part needs thickness, stiffness or a sealing face that bending cannot hold.

For early design work where the geometry is still moving, 3D printing gives a physical part in a day. Switch to CNC machining once the interfaces are frozen, because that is when tolerance and material properties start to matter. Running both in parallel on the same revision is a common and sensible split.