Basic Knowledge of CNC Mill

A 3-axis mill moves the table in X and Y and the spindle in Z. The cutter approaches the part from one direction only, so every pocket, bore and slot on that face can be cut in a single setup. Flip the part and you need a second setup, a second zero point, and a second chance to introduce stack-up error.

Adding a fourth axis puts a rotary table under the work. The part can now index to 90° or 45° positions without being unclamped. That one change removes several setups on parts with features on multiple sides, such as a manifold block with ports on four faces. GreatLight runs 12 four-axis mills and a Ø400 mm rotary table for this class of work.

Five-axis machining adds tilt on top of rotation. The tool can stay normal to a curved surface instead of dragging across it, which improves finish on contoured geometry and lets short, stiff cutters reach deep pockets. We keep 16 simultaneous 5-axis machining centers for impellers, aerospace brackets and medical housings where the geometry cannot be reached any other way.

Not every part needs more axes. A flat plate with holes on one face is cheaper and faster on a 3-axis machine. Move up an axis only when the drawing forces it.

• 1
  3-axisSingle-face work, flat plates, simple pockets. Lowest setup cost.
• 2
  4-axisFeatures on multiple sides, cylinders with cross holes, indexing work.
• 3
  5-axisContoured surfaces, deep cavities, undercuts, one-setup complex parts.

A flat end mill leaves a square internal corner with a radius equal to the tool radius. Designers often forget this. A 6 mm cutter cannot produce a sharp 90° corner at the bottom of a pocket. It leaves a 3 mm radius. Draw the radius you can live with, or accept that the corner will be finished by EDM or a broach.

Ball nose cutters are used for 3D contouring. They leave a scalloped surface, and the stepover controls the scallop height. A 0.2 mm stepover on a 10 mm ball cutter gives roughly Ra 0.8 μm on aluminum. Increase the stepover to 1 mm and the finish drops to around Ra 3.2 μm. Polishing can close the gap but adds cost.

Drills, reamers and taps each have their own place. A reamed hole holds ±0.005 mm and a fine bore finish. A drilled hole is typically ±0.05 mm and Ra 1.6–3.2 μm as machined. If the drawing calls for an H7 fit, reaming or boring is mandatory. The drill is only the pilot.

Tool reach matters more than diameter. A long, thin cutter deflects under load, and the deflection shows up as taper in the wall. The rule of thumb: keep the flute length under 4× the diameter. Beyond that, expect to slow the feed and take lighter passes.

A vise is the default for prismatic parts. It is fast, repeatable and cheap. The limit is access. A vise jaw blocks the bottom face and often part of a side, so features there need a second operation. Soft jaws machined to the part profile hold better and mark less, which matters on finished surfaces.

Fixtures make sense when the part is thin, flexible or has no parallel faces. A plate 2 mm thick will chatter in a vise no matter how gently you cut it. A vacuum plate or a bed of sacrificial material supports the whole face and lets the cutter run at normal speeds. This is common on electronics enclosures and heat sinks.

For 5-axis work, a trunnion or a zero-point clamping system holds the part off the table so the tool can reach underneath. The trade-off is rigidity. A part on a tall tombstone vibrates more than the same part in a vise. Keep the overhang short and the cutter sharp.

Clamping marks are a real cost. If a face is cosmetic, plan a light finishing pass after the clamps move, or design a clamping tab that gets cut off later.

A milling machine can hold ±0.005 mm on a good day, but that number applies to a specific feature under specific conditions. Thermal growth, tool wear and fixture deflection all eat into it. On a 300 mm aluminum part, a 5 °C shop temperature swing moves the part by roughly 0.02 mm. We control shop temperature, but the part still grows when it leaves the machine.

Surface finish and tolerance compete. A fine Ra 0.2–0.8 μm finish needs a small stepover and a sharp tool, which slows the cycle. A standard as-machined Ra 1.6–3.2 μm finish runs faster and costs less. Specify the finish only where it matters. A sealing face needs Ra 0.8 μm. A mounting bracket does not.

Inspection closes the loop. We check raw material on arrival, monitor dimensions in process, and inspect 100% before shipment. Reports are available on request. If a drawing calls for a CMM report on every part, say so at quote time. It changes the plan.

The most common tolerance mistake is over-specifying. A ±0.01 mm callout on a non-functional surface adds cost and inspection time for no benefit. Ask what the feature does before you tighten the number.

Aluminum 6061-T6 is the default for prototypes and many production parts. It cuts fast, holds a good finish and takes anodizing well. 7075 is stronger but gummier, so feeds and speeds drop. 2024 machines cleanly but has poor corrosion resistance without a coating. We keep all three in stock.

Stainless 303 is the free-machining grade and the easiest to turn and mill. 304 and 316 work-harden if the cutter rubs, so the feed must stay aggressive. 17-4PH (SUS630) machines in the annealed state and then ages to high strength. If the drawing specifies 316L for a medical part, expect slower cycle times and more tool wear than 303.

Steel 1018 and 1045 are common for structural parts. 4140 and 4340 are used when strength matters and are usually heat treated after machining. Tool steel above 50 HRC is not a milling job. It goes to EDM or grinding. We route those parts accordingly.

Titanium TC4 (Ti-6Al-4V) and Inconel are aerospace materials. They conduct heat poorly, so the cutter takes the heat and wears fast. Speeds drop to a fraction of aluminum. These parts need rigid setups and fresh tooling, which affects both cost and lead time.