Machining parts: how CNC removal works and where it stops

• 1
  What actually happens at the cutting edge
• 2
  Why ±0.005 mm is a process claim, not a wish
• 3
  Undercuts, deep pockets, and the reach problem
• 4
  When a lathe beats a mill
• 5
  Material drives the cutting parameters, not the other way around
• 6
  Which process fits the part

Every machining part starts as a solid block, bar, or plate. A rotating cutting tool is driven along a programmed path, and the material that is not the part is turned into chips. Nothing is formed or added, so the final geometry is bounded by what a tool can physically reach.

The tool does not cut freely. It is pushed into the material, and the material pushes back. That force deflects the tool, the holder, and the workpiece. On a slender 6 mm end mill sticking 40 mm out of a holder, deflection is often the largest single source of dimensional error, not the machine's positioning accuracy.

Heat is the second constraint. Aluminium 6061 conducts heat away quickly and machines at 3,000–8,000 rpm with high feed rates. Titanium TC4 (Ti-6Al-4V) conducts heat poorly, so the edge temperature climbs and the tool wears fast. That is why titanium machining parts run at 40–80 m/min surface speed instead of the 300–500 m/min used on aluminium.

Chip evacuation decides whether a deep pocket succeeds. If chips recut, the edge dulls and the wall finish drops to Ra 3.2 μm or worse. Through-spindle coolant and pecking cycles fix most of it. The rest is toolpath choice.

Tolerance is the total window a dimension may occupy. On a machining part, that window is filled by machine positioning, thermal drift, tool wear, workholding deflection, and measurement uncertainty. Each term is small. Their sum is not.

A machine that positions to ±0.002 mm still cannot hold ±0.005 mm on a thin wall if the wall moves 0.02 mm when the vise releases. Stress relief matters too. A 7075 block machined straight from the plate will move after the first heavy pass, and the second setup cuts into a shape that already changed.

Temperature is the quiet one. A 100 mm aluminium part grows about 0.0023 mm per 1 °C. A shop floor that swings 6 °C between morning and afternoon shifts the part by roughly 0.014 mm before the tool touches it. Climate control is not a luxury at this tolerance.

So when we quote ±0.005 mm, we mean it on features we can reach in one setup, in a temperature-controlled cell, on material that has been stress-relieved. Deep bores, long thin shafts, and thin floors usually need a wider window or an intermediate semi-finish pass.

A 3-axis machine moves the tool in X, Y, and Z. The part sits still. Any feature that faces away from the spindle axis cannot be reached without turning the part by hand and re-datuming it. That is a setup, and each setup adds error.

A 5-axis machine tilts the tool or the table, so the cutting edge can meet a compound angle in one setup. On a machining part with ports on five faces, that can remove three or four setups. Fewer setups mean tighter true position between features, because the same datum chain holds throughout.

Reach is the hard limit, not axis count. A pocket 80 mm deep with a 20 mm corner radius needs a tool long enough to get down there. A long tool chatters. If the drawing calls for Ra 0.8 μm on those walls, the answer may be a smaller tool with a smaller corner radius, or electrical discharge machining instead.

Undercuts are the classic no. A groove wider at the bottom than the opening cannot be cut by a tool entering from that direction. Either the designer opens the geometry, or the part splits into two pieces, or the process changes.

Turning spins the workpiece against a single-point tool. Any part that is mostly a body of revolution, such as a shaft, bushing, flange, or fitting, belongs on a lathe. Material removal is continuous, so cycle time is short and surface finish is easy to hold at Ra 0.8–1.6 μm without a second operation.

Milling cuts with a multi-tooth tool on a stationary part. Prismatic shapes, pockets, slots, and flat faces belong here. A mill-turn center does both on one platform, which matters on a machining part like a hydraulic manifold that has a turned spigot and a milled port face that must stay concentric.

The decision is rarely about which process is better. It is about which one reaches the critical feature with fewer setups. If the tightest tolerance is on a diameter, turn it. If it is on a bolt pattern, mill it. If it is on both, that is what mill-turn is for.

One practical rule: keep turned features and milled features on separate datums in the drawing, and note which one controls. That single note prevents most of the back-and-forth during first-article inspection.

Aluminium 6061-T6 is the default for machining parts that need to be stiff, light, and anodized. It cuts fast, holds tolerance well, and welds. 7075 is stronger but less corrosion-resistant and more prone to residual stress. 2024 machines cleanly but is difficult to weld.

Stainless 303 is the free-machining grade and turns beautifully. 304 and 316 gum up more, work-harden if the tool rubs, and need constant feed to stay under the hardened layer. 17-4PH (SUS630) machines in the solution-treated state and then ages to high strength, which is useful when the part must stay dimensionally stable after heat treatment.

Steel 1018 and 1045 cover most general shafts and plates. 4140 and 4340 are for loaded parts. Tool steel is for dies and wear surfaces. Inconel and titanium TC4 sit at the hard end: slow speeds, heavy coolant, sharp edges, and a willingness to change tools before they fail.

Plastics are their own discipline. POM and HDPE cut cleanly but move with temperature. PEEK needs sharp tooling and slow feed or it burns. Carbon fibre machines as a composite, so the tool wears on the fibre, and the dust needs extraction. A drawing that specifies Ra 0.8 μm on POM will be hard to meet and harder to measure.