What Can Be Done With a CNC Machine?

• 1
  What is done with a CNC machine: four core operations
• 2
  Milling, turning, and the geometry each one owns
• 3
  Materials a CNC machine cuts well, and the ones that fight back
• 4
  Tolerance, finish, and what actually drives cost
• 5
  When a CNC machine is the wrong choice
• 6
  Which process fits which part

Nearly every machined part comes from one of four operations: milling, turning, drilling, and the secondary work that follows. Milling rotates a cutter and moves it through a stationary block. Turning spins the workpiece against a single-point tool. Drilling makes holes, then boring or reaming brings them to size. A CNC machine reads coordinates from a program, so the same motion repeats on part 1 and part 10,000.

That repeatability is the real answer to what is done with a CNC machine. The toolpath is fixed in code. Once the first article is inspected and approved, the machine holds ±0.005 mm on features that fit inside its work envelope. On our 16 simultaneous 5-axis centers, that envelope reaches 4,000 × 400 × 150 mm for long parts and 750 × 1,150 × 550 mm for plate work.

The process is subtractive, so it starts from solid stock. Bar, plate, extrusion, or casting goes in; a finished part comes out. There is no mold to cut and no tooling cost to amortize, which is why one prototype and a 10,000-part run use the same setup logic. The difference is fixture design and cycle time, not the principle.

The limits are physical, not conceptual. A cutter must reach the feature. A tool must be rigid enough to cut without chatter. A part must be held without deforming. Where any of those three fail, the design needs a different process or a redesign. Most manufacturability problems trace back to one of them.

Milling owns prismatic geometry: pockets, slots, bosses, faces, and contoured surfaces. A three-axis mill cuts from one direction, so every feature must be reachable from the top. Undercuts and side-wall holes need a fourth axis, which tilts the part or rotates it between setups. We run 27 three-axis machines and 12 four-axis mills for exactly this split.

Turning owns rotational geometry: shafts, bushings, fittings, and threaded bodies. The workpiece spins and a single-point tool follows the profile. Diameters hold tighter than milled features because the cut is continuous. Mill-turn centers combine both, so a part like a valve body can be turned and then cross-drilled in one setup. We run 16 of them.

Five-axis machining adds two rotary axes to the mix. The tool can approach a surface at an angle instead of straight down. That lets a ball-nose cutter engage the flank rather than the tip, which improves surface finish and extends tool life. It also reaches features that would need three separate fixtures on a three-axis machine.

The gain is not just access. Fewer setups mean fewer datum shifts. Each re-fixturing adds stack-up error, typically 0.01–0.03 mm per move. On a part with tight true position between two faces, cutting both in one five-axis setup removes that error entirely. That is the main reason complex parts migrate to five axes.

• 1
  3-axisFlat plates, covers, brackets, simple pockets
• 2
  4-axisCylindrical parts with cross features, multi-face holes
• 3
  5-axisContoured surfaces, undercuts, tight true position
• 4
  Mill-turnRotational body plus off-axis drilling in one setup

Aluminum is the default for prototypes and housings. 6061-T6 cuts fast, holds ±0.005 mm, and anodizes cleanly. 7075 is stronger but gummier, so it needs sharper tools and lighter depths of cut. 2024 machines well but has poor corrosion resistance without coating. All of these are routine work.

Stainless grades split by machinability. 303 and 304 turn and mill predictably. 316L is tougher and work-hardens if the tool dwells, so feed rates stay high and radial engagement stays light. 17-4PH machines in the annealed state and then ages to high strength. 440C is hard and abrasive, so tool life drops and cost rises.

Titanium and nickel alloys are where cost jumps. Ti-6Al-4V conducts heat poorly, so the cutting edge absorbs it. Speeds drop to roughly a quarter of aluminum, and cutters wear faster. Inconel is worse. These materials are still machinable, but the cycle time and tooling cost are part of the quote, not a surprise.

Plastics behave differently. POM and ABS cut cleanly with sharp tooling and air blast. PEEK and PC need stress relief and careful clamping because they deflect under cutting force. Carbon fibre is abrasive and delaminates if the fiber direction is ignored. Each has a workable window, but the window is narrower than metal.

• 1
  Easy6061, 6082, brass C36000, POM, ABS
• 2
  Moderate304, 316L, 4140, 17-4PH, PEEK
• 3
  DifficultTi-6Al-4V, Inconel, 440C, magnesium

Tolerances below ±0.005 mm are possible on small features but need temperature control, sharp tooling, and in-process gauging. Every feature tightened to that band adds inspection time. A part with two critical dimensions is cheap to verify. A part with forty is not. Designers who tag every dimension as critical pay for all of them.

Surface finish follows the same logic. As-machined surfaces land at Ra 1.6–3.2 μm. A finish pass brings that to Ra 0.8–1.6 μm. Fine finishes at Ra 0.2–0.8 μm need slower feed, smaller stepover, and often a dedicated finishing tool. The jump from Ra 1.6 to Ra 0.4 can double cycle time on a contoured face.

Feature depth matters more than feature size. A pocket 4× deeper than its width needs a long, thin cutter that deflects and chatters. The usual fix is a larger corner radius on the tool, but that leaves a larger internal radius in the pocket. If the drawing calls for a sharp internal corner, the part needs EDM or a design change.

Setup count is the quiet cost driver. Each additional orientation means a new fixture, a new datum, and a new chance for stack-up error. Parts designed so all critical features face one direction machine in one operation and ship faster. Parts that need five faces touched need more of everything.

CNC machining loses on unit cost once volume is high and geometry is simple. A die-cast housing at 50,000 units costs a fraction of a machined one. The crossover sits somewhere in the low thousands for most parts, and it moves with part size and feature count. Below that, machining wins because there is no tooling to pay for.

It also loses on internal geometry. A hollow channel inside a solid block cannot be cut by a rotating tool. Additive processes build those channels. The practical answer is often hybrid: print the manifold, machine the sealing faces. Neither process alone gets there cleanly.

Very thin walls are another boundary. Aluminum below about 0.8 mm deflects under clamping and cutting force. The part may measure correctly on the bed and spring out of tolerance once unclamped. Thicker walls or a stress-relief step between roughing and finishing solves it, at added cost.

Hardened material above roughly 45 HRC is usually ground rather than milled. A CNC machine can cut it with ceramic tooling, but the finish and tool life are worse than grinding. If the part is already heat treated, check whether grinding is the cheaper route before assuming it must be milled.