CNC machining briefly explained

• 1
  CNC machining briefly explained: what happens inside the machine
• 2
  Three axes, four axes, five axes: where the boundary sits
• 3
  What the geometry must allow
• 4
  How tolerance and finish drive the process
• 5
  When CNC machining is the wrong choice
• 6
  Material choice changes the cutting conditions
• 7
  What the shop needs to quote accurately
• 8
  Choosing the machine configuration

CNC machining is subtractive. A CAM programmer converts a 3D model into tool paths, and the controller drives a spinning cutter along those paths to remove material from a solid block. The block may be aluminium plate, stainless bar, titanium forging or a plastic billet. Nothing is formed or added, so the final shape depends entirely on where the cutter was told to go.

Every cut has three numbers behind it: spindle speed, feed rate and depth of cut. A 12 mm carbide end mill in 6061 aluminium might run at 3,000–6,000 rpm with a 0.5–2.0 mm radial stepover. The same cutter in 316 stainless drops to roughly 600–1,200 rpm and a much lighter stepover. Get these wrong and you get chatter, tool wear or a scrapped part, not a slow part.

The cutter leaves marks. A sharp tool at a light stepover leaves a smoother floor than a worn tool pushed hard. That is why surface finish is quoted as a range such as Ra 1.6–3.2 μm as machined, or Ra 0.8–1.6 μm when the finish matters. Finish is a machining decision, not a coating decision.

Heat is the quiet constraint. Aluminium carries heat away with the chip. Titanium holds heat at the cutting edge, so speeds stay low and coolant flow matters more. This is the first place a design either helps the shop or fights it.

A three-axis machine moves in X, Y and Z only. The tool always comes down from the same direction, so every feature must be reachable from that direction. For a plate with pockets, holes and a flat profile, three axes is fast, stable and cheap. If your part is prismatic, stop reading here and quote it as 3-axis.

A fourth axis adds rotation around one axis, usually A. The workpiece can be indexed to four sides without being unclamped. This suits parts with features on multiple faces, such as a manifold block with ports on three sides. You get fewer setups, which means better position accuracy between features.

Five-axis adds two rotary axes, so the tool can tilt relative to the workpiece. The real gain is not just reach. It is that a ball-nose cutter can stay normal to a curved surface, which lets one tool cut a contoured face to a good finish instead of leaving scallops. It also lets a short, stiff cutter reach deep features that would need a long, flexing tool on a 3-axis machine.

The trade-off is real. Five-axis setups take longer to program and prove out, so the hourly cost is higher. When a part is simple, that cost buys nothing.

A cutter is a cylinder with a limited length-to-diameter ratio. A pocket 4× deeper than the cutter diameter will chatter or need a reduced stepover. A pocket 8× deeper usually needs a smaller tool, a longer reach and a lot of patience. If a deep pocket is not functionally necessary, make it shallower and the part gets cheaper.

Internal corners cannot be sharper than the cutter radius. If a drawing calls for a square internal corner, the shop either leaves a radius or adds an EDM step. Specify the largest radius the function allows, and say so on the drawing.

Wall thickness matters too. Thin walls deflect under cutting force, so they come out tapered or with chatter marks. In aluminium, walls under 0.8 mm get difficult. In stainless or titanium, the floor is higher. Add a temporary rib or accept a slower pass.

Threads, holes and slots all have standard tooling behind them. A hole called out at Ø6.35 mm may need a drill and a reamer; a hole at Ø6 mm can often be drilled and bored with one setup. Slight changes to nominal sizes can remove an operation.

Tolerance is where cost concentrates. A general tolerance of ±0.1 mm on a milled aluminium part is routine. Tightening a critical bore to ±0.005 mm means the machine must be thermally stable, the tool must be new, and the part may need to be measured and adjusted mid-run. That is a different job, not a tighter note on the same drawing.

Not every dimension needs the tight number. If a bore locates a bearing, tighten that bore. If a clearance hole passes a screw, leave it loose. Mixed tolerances are normal and expected; a drawing where every dimension is ±0.01 mm tells the shop the designer did not decide which features matter.

Surface finish follows the same logic. Ra 3.2 μm is fine for a bracket. Ra 0.8 μm or better is needed for a sealing face, a sliding surface or a mating face that must not leak. Finer finishes usually mean a finishing pass with a smaller stepover, which adds time.

Measurement is part of the process, not an afterthought. A ±0.005 mm callout implies a CMM or a high-accuracy gauge, and that inspection time belongs in the quote.

CNC is not always the answer. For a hollow shell or a complex internal channel, machining from solid wastes material and time. Die casting or vacuum casting produces the near-net shape, then machining finishes only the critical faces. For a thin-walled enclosure in volume, sheet metal fabrication is usually faster and cheaper.

For a lattice, a ducted internal passage or a part with many small identical features, additive processes can build geometry that no cutter can reach. Machining can still finish the mating surfaces afterward.

There is a size ceiling too. Our largest travel is 4,000 × 400 × 150 mm, and rotary work fits a Ø400 mm table. Parts larger than that need to be split or made another way.

The honest rule: if the part is mostly solid and its features are reachable from a few directions, machining wins. If the part is mostly empty space, another process probably wins.

Aluminium 6061-T6 is the default for prototypes and fixtures. It machines fast, holds tolerance well and anodizes cleanly. 7075 is stronger but less forgiving, and it is common in aerospace brackets. 2024 machines well but has poor corrosion resistance without a coating.

Stainless 303 is the free-machining grade and the easiest in the family. 304 and 316 work-harden, so the cutter must keep moving and never rub. 17-4PH machines in the annealed state and is then aged to high strength, which suits aerospace and medical parts.

Titanium Ti-6Al-4V and Inconel are slow. Tool life is short, speeds are low and the material cost is high, so the design should remove as few cubic centimeters as possible. A near-net forging is often cheaper overall than a block.

Plastics behave differently again. POM and PEEK machine cleanly; ABS and PP can melt or burr if the cutter dwells. Carbon fibre is abrasive and dulls tooling quickly, so it is usually cut with diamond-coated tools.

A STEP file gives geometry. A PDF drawing gives intent. Send both, and send them together. If the two disagree, the shop has to guess.

Mark the critical dimensions. If a bore, a flatness callout or a surface finish is functional, say so. If everything is marked critical, nothing is, and the quote will assume the worst case.

State the quantity and the stage. A one-off prototype and a 10,000-part run are quoted differently, and features that are expensive at one piece may be cheap at volume once a fixture exists.

Finally, state the application. A part that goes into a medical device or an automotive assembly carries documentation and traceability requirements that change the workflow. Knowing the end use up front avoids a second quote later.