CNC Manufacturing: How Metal Removal Actually Works

• 1
  What CNC Manufacturing Does Where the Tool Meets the Part
• 2
  Which Tolerance Actually Reaches the Drawing
• 3
  Surface Finish Follows the Toolpath
• 4
  Setup Count Drives the Price of CNC Manufacturing
• 5
  Material Choice Sets the Floor on Feeds and Speeds
• 6
  Process Fit by Part Characteristic

CNC manufacturing is subtractive. A rotating cutter is driven along a programmed path, and every point on that path removes material. The machine does not know what the part is. It only knows coordinates, feed rate, spindle speed, and where the tool tip sits relative to the workpiece.

That is why the first engineering question is never "can it be machined" but "can the tool reach the feature". A pocket 8 mm deep and 6 mm wide needs a cutter smaller than 6 mm, and a 5 mm cutter can only reach about 25 mm before it deflects. Deep, narrow, sharp-cornered geometry is where quotes climb.

Material comes off as chips, and chips carry heat away. Cut too conservatively and the tool rubs instead of cutting, which work-hardens stainless and burns the edge. Cut too aggressively and the tool deflects, leaving taper in the wall. The window between those two failures is the cutting data a shop has already dialed in for each material.

Tool pressure pushes the part, the fixture, and the tool at the same time. On a thin wall, that force bends the workpiece away from the cutter, so the finished wall is thicker at the bottom than at the top. Rough the wall, let it spring back, then take a light finishing pass. That is a process decision, not a drawing decision.

A general title-block tolerance of ±0.1 mm is cheap. It lets the shop choose feeds and fixtures freely and inspect with calipers. When a feature is called out at ±0.005 mm, the shop has to control temperature, tool wear, and clamping force, and it has to measure with a coordinate measuring machine rather than a caliper.

The cost is not linear. Going from ±0.1 mm to ±0.05 mm is a small step. Going from ±0.05 mm to ±0.005 mm changes the machine, the fixture, and the inspection method. Put the tight callout only on the features that need it: a bearing bore, a mating face, a seal groove.

Datums matter more than the number. If a hole position is called from three different faces, the inspector cannot reproduce the setup the machinist used. Pick one primary datum, one secondary, one tertiary, and locate everything from that frame. Fewer setups also mean fewer chances to stack error.

Some tolerances cannot be held by cutting at all. A Ø6 H7 bore in a 300 mm long aluminum tube will move after machining as residual stress releases. Rough it, stress-relieve it if the alloy allows, then finish. If the tolerance still will not hold, that is a sign the feature belongs in a different process.

Surface roughness comes from the scallop left between passes. A 12 mm ball cutter stepping over 0.2 mm leaves a shallower scallop than a 6 mm cutter stepping over the same 0.2 mm. Stepover, tool radius, and feed per tooth set the arithmetic; the operator chooses the numbers.

Ra 1.6–3.2 μm is as-machined and covers most brackets, housings, and plates. Ra 0.8–1.6 μm needs a finishing pass with a sharp insert and a stable setup, and it is the usual target for sealing faces and sliding surfaces. Ra 0.2–0.8 μm is a polishing or fine-boring operation and should be reserved for optical, vacuum, or bearing-grade surfaces.

Direction matters as much as the number. A surface that slides against a seal wants the tool marks running around the bore, not across it. Add a note like "circumferential finish" or the shop will pick the cheaper path.

Finish also changes with material. Aluminum 6061 cuts to a bright surface easily. 304 stainless work-hardens under a dull tool and tears. Titanium Ti-6Al-4V needs low cutting speed and plenty of coolant, or the edge chips and the finish goes with it.

Every time the part is unclamped and turned, the operator re-establishes zero and the part accumulates a new error. A part machined on five faces in three setups costs more than the same part machined in one setup on a 5-axis center, even when the cutting time is identical.

This is why 5-axis work is not automatically expensive. For a complex bracket with angled faces and holes, one 5-axis setup can replace three 3-axis setups. Fewer setups also mean fewer fixtures to design and build, which is often the larger cost on a low-volume run.

For parts that are long and shallow, a 4,000 × 400 × 150 mm travel machine can hold the whole part in one setup. A 4,000 mm shaft or rail does not need to be repositioned mid-cut, so straightness stays inside the tolerance without a second operation.

Fixtures are the hidden line item. Soft jaws, vacuum plates, and custom clamps all cost money and lead time. If a design can be held on a standard vise or a faceplate, say so. Design the part around the fixturing you can imagine, not just the geometry you need.

Aluminum 6061 and 7075 machine fast and hold tight tolerances well. 7075 is stronger but more prone to stress movement after roughing, so leave stock and finish after a pause. 2024 behaves similarly. Cast alloys like ADC12 cut easily but can have porosity that shows up as a pit after anodizing.

Stainless 303 is the free-machining grade and the right default for turned parts. 304 and 316 are tougher, gummier, and more prone to work hardening; they need sharp tools and constant feed. 17-4PH machines well in the annealed condition and gains strength after heat treatment.

Steel 1018 and 1045 are straightforward. 4140 and 4340 are used for shafts and tooling where strength matters; pre-hardened 4140 at 28–32 HRC is still machinable but slower. Tool steels should be machined before hardening whenever the geometry allows.

Titanium and Inconel are the slow end. Ti-6Al-4V conducts heat poorly, so the cutting edge runs hot; speeds drop to a fraction of aluminum and tool life is short. Inconel is worse. These materials are machined when nothing else meets the service condition, not to save money.

Plastics behave differently again. POM and PEEK hold tolerance well but move with temperature. ABS and PC are soft and can be scratched by chip evacuation. Carbon fibre wears tools fast and needs dust control.