What Can CNC Machines Do?

• 1
  What CNC machines do: controlled metal removal
• 2
  Shapes and features CNC machining handles well
• 3
  Which materials cut well and which fight back
• 4
  Tolerances, surface finish and where they get expensive
• 5
  From one prototype to a 10,000-part run
• 6
  What happens after the cut
• 7
  What each machine configuration can do
• 8
  When CNC machining is the right call and when it is not

A CNC machine does one physical thing: it moves a sharp edge through material along a path that a program defines. A controller reads G-code, closes the loop on servo position, and drives ball screws and linear guides so the tool tip travels the same path on part 1 and part 10,000. Everything else engineers talk about, such as flatness, hole position and surface finish, follows from that repeatability.

Two families cover most work. Milling spins a multi-flute cutter and moves it in X, Y and Z, so the tool sweeps a volume out of a solid block. Turning spins the workpiece against a single-point insert, so material goes away as a continuous chip on a rotating diameter. A mill-turn center does both in one setup, which matters when a part has a turned bore and milled flats that must stay concentric.

The cut itself is a controlled fracture. Each flute bites a chip of defined thickness, and the heat leaves mostly with that chip. Feed per tooth, spindle speed, radial engagement and coolant decide whether the edge slices or rubs. Rubbing work-hardens stainless and burns the insert, so feeds that look conservative often cost more than they save.

• 1
  Milling removes volumeRotating cutter, stationary work, best for pockets and profiles
• 2
  Turning removes diameterRotating work, single-point tool, best for shafts and bores
• 3
  Mill-turn combines bothFewer setups, tighter concentricity between features

Prismatic parts with pockets, ribs, bosses, slots and drilled hole patterns are the natural fit. A three-axis mill reaches every face that points up, so a part with features on one side, or on two sides separated by a flip, machines quickly and cheaply. Positional accuracy is limited mainly by the fixture and the tool, not the control.

Five-axis work changes the reachable set. Two extra rotary axes tilt the tool or the table, so undercuts, deep cavities, angled faces and blended surfaces get cut in one setup. On a 16-machine bank of simultaneous five-axis centers we hold ±0.005 mm (±0.0002 in) on production parts, and the real gain is not only the tolerance but the removal of re-fixturing error between operations.

Some geometry still resists. A deep narrow slot narrower than the smallest available cutter cannot be milled, because the tool shank rubs the wall before the tip reaches depth. Sharp internal corners cannot be cut by a round tool; the corner radius equals the cutter radius, so design a relief or accept the radius. Blind holes need a drill point angle unless they are flat-bottomed by a separate tool.

• 1
  Good fitPockets, ribs, hole patterns, contoured surfaces, turned diameters
• 2
  Needs five axesUndercuts, deep angled cavities, blended freeform faces
• 3
  Poor fitSlots below tool diameter, true sharp internal corners, deep thin walls

Aluminium is the easy case. Grades 6061 and 7075 cut at high spindle speeds, hold ±0.005 mm without drama, and take anodizing well. 7075 is stronger but gummier, so use sharper geometry and more coolant. Cast grades such as ADC12 machine freely but can hide porosity that shows up after anodizing, which is why we check raw material before a run.

Stainless 303 and 304 turn cleanly with the right feeds. 316L and 17-4PH work-harden if the tool rubs, so keep the chip load up and never dwell in the cut. Titanium TC4 (Ti-6Al-4V) and Inconel cut hot and slow; tool life is short, and thin walls deflect. These parts are machinable but the cost sits in cycle time and cutter replacement, not in the machine hour.

Plastics behave differently again. POM and ABS cut fast and burr lightly. PEEK and carbon fibre need sharp, uncoated tooling and dust extraction. Carbon fibre is abrasive and eats carbide edges, so plan for more than one cutter per part. Copper alloys such as C36000 machine freely; pure C110 copper is gummy and needs high rake angles.

The material list is wide, but the decision rule is simple. If the alloy work-hardens, keep the tool moving and the chip thick. If it conducts heat poorly, flood the cut. If it is abrasive, budget for tool wear in the quoted price.

• 1
  Free cutting6061, 2024, 303, C36000 brass, POM, ABS
• 2
  Work hardening304, 316L, 17-4PH, Inconel
• 3
  Abrasive or heat sensitiveTC4 titanium, carbon fibre, PEEK

Tolerance is a cost curve, not a checkbox. A general machining tolerance of ±0.1 mm is easy on most features. Squeezing to ±0.005 mm needs the right machine, a rigid fixture, temperature control in the shop, and in-process gauging. The tighter the callout, the more of the part price is inspection rather than cutting.

Surface finish follows a similar rule. As-machined surfaces land around Ra 1.6–3.2 μm. A finer pass with a smaller stepover reaches Ra 0.8–1.6 μm. Below Ra 0.2–0.8 μm you are usually looking at a finishing operation, not a different cutter path, and polishing or lapping becomes part of the process plan.

Not every dimension deserves a tight number. Datum features, bearing bores and mating faces justify ±0.005 mm. A clearance hole for an M6 screw does not. Marking tight tolerances on non-functional features raises the price and can push the shop into extra setups that add error rather than remove it.

Every part ships after 100% inspection, with raw material checks before the run, monitoring during it and a final inspection before packing. Reports are available on request. If a drawing calls for a tolerance the process cannot hold, the honest answer is a design change, not a promise.

• 1
  Loose±0.1 mm on clearance holes and non-mating faces
• 2
  Standard precision±0.005 mm on datums, bores and mating surfaces
• 3
  Fine finishRa 0.2–0.8 μm usually means a secondary operation

The same program that cuts a prototype cuts the production part. That is the practical advantage of CNC for product teams: the first article is made from the final material with final tolerances, so fit and function tests mean something. No tooling waits in between.

For small batches, no minimum order quantity applies. A single prototype and a 10,000-part run use the same fixturing logic; only the workholding and inspection plan change. Production can start within 24 hours of a released drawing, and parts typically ship in 3–5 days.

Large runs change the economics. Cycle time per part, tool wear and fixture design dominate the price. A dedicated fixture that holds six parts per load can cut the machine hour per part, while a soft jaw setup for one part keeps the unit price high. It pays to ask what the fixture plan is before comparing quotes.

Long parts are a separate constraint. The largest travel on our machines is 4,000 × 400 × 150 mm, with medium envelopes of 750 × 1,150 × 550 mm and 600 × 600 × 600 mm, and compact cells at 500 × 500 × 450 mm and 500 × 310 × 200 mm. If a part is longer than the travel, the design has to be split or the process changed.

• 1
  PrototypeFinal material, final tolerance, no tooling wait
• 2
  Small batchNo minimum order quantity, same program
• 3
  Large runFixture plan and cycle time set the unit price

A machined part is rarely ready to bolt on. Burrs sit on every edge that left a cutter, and sharp edges are a handling and fit problem. Bead blasting, tumbling and brushing remove them and set a uniform cosmetic surface. Tumbling is cheap and rounds edges slightly; bead blasting gives a matte finish but can hide fine detail if the media is coarse.

Coatings change dimensions, and the drawing should say so. Anodizing builds an oxide layer that grows into the surface and out of it, so a hardcoat on a tight bore can close the fit. Electroless nickel and zinc plating add a measurable thickness on every face. If a thread or bore must stay on size, mask it or cut it undersize before plating.

Functional finishes matter as much as cosmetic ones. Conductive anodizing keeps grounding paths alive. Black oxide holds oil on steel but offers limited corrosion protection on its own. Powder coating is thick and hides machining marks, which is fine for a bracket and wrong for a sealing face.

Laser marking is the last step. Minimum character height is 1.5 mm for a clean read. Part numbers, revision codes and traceability marks go on a face that will not be machined again and will not sit against a mating surface.

• 1
  Deburr and cosmeticBead blasting, tumbling, brushing, polishing
• 2
  Protective and conductiveAnodizing, electroless nickel, zinc, black oxide
• 3
  TraceabilityLaser marking, minimum character height 1.5 mm