Aircraft CNC machining: the art of precision cutting

Precision cutting is subtractive work under numeric control. A CAM programmer takes your solid model, picks toolpaths, and posts code that the machine follows without an operator turning handwheels. On a 3-axis mill the cutter moves in X, Y and Z only. Add a fourth axis and the part rotates; add a fifth and the tool can tilt, so undercuts and compound angles get cut in one setup.

The sequence matters more than the machine. We face the stock, establish a datum, then rough with the largest rigid tool that fits. Semi-finish removes the stair-steps left by the rougher. Finish cuts run at light radial engagement and higher spindle speed to hold surface finish and wall straightness. On thin ribs, we leave material and take it off in a second pass after stress has moved.

Code alone does not hold a tolerance. Fixturing does. A part that springs 0.05 mm when unclamped will not pass a first-article check even if the cutter was perfect. For aircraft work we prefer soft jaws machined to the part profile, vacuum plates for thin plate, and sacrificial tabs on parts that would otherwise chatter.

Chip control is a real constraint on aluminium and titanium. Deep pockets need through-spindle coolant or air blast, and peck cycles that clear chips instead of recutting them. Recut chips are the most common cause of a torn finish and a scrapped pocket floor.

• 1
  Rough with rigid toolsLarge diameter, short gauge length, high material removal rate.
• 2
  Semi-finish before finishLeaves a uniform stock allowance so the finisher cuts steady load.
• 3
  Control the clampSoft jaws or vacuum so release does not move the part.
• 4
  Clear the chipsThrough-tool coolant or air on deep pockets and titanium.

We hold ±0.005 mm (±0.0002 in) on features that need it. That number is not a default. Applying it to every dimension on a bracket triples the cost and adds nothing, because the assembly only locates on two or three features. Mark the functional interfaces tight and let everything else run general tolerance.

Surface finish follows the same logic. A sealing face or a bearing bore may need Ra 0.2–0.8 μm. A non-critical web can run as-machined at Ra 1.6–3.2 μm. Between those, Ra 0.8–1.6 μm covers most mating surfaces. If you call out a fine finish everywhere, someone has to spend time with a small stepover that could have gone into a stiffer setup.

Datums drive inspection. If the drawing calls out A, B and C, the fixture has to present those three surfaces the same way the CMM will. When a datum is a hole pattern rather than a face, we sometimes drill and ream the pattern first, then use it to locate the rest of the part. That keeps the tolerance stack honest.

Thermal drift is small at these sizes but real. Titanium and aluminium expand at different rates, and a part measured on the machine at 28 °C can measure differently in a 20 °C inspection room. For tight bores we let the part stabilize before final inspection rather than trusting an in-process number.

Aluminium 7075 cuts clean and holds a sharp edge, which is why it shows up in brackets and fittings. It is also notch sensitive and does not like being clamped hard. 6061-T6 is easier to machine and weld, better for housings and non-structural frames. 2024 sits between them and machines well but has poor corrosion resistance without coating.

Titanium Ti-6Al-4V (TC4) is the material most people underestimate. It conducts heat poorly, so the cutting edge absorbs it. Speeds drop, tool life drops, and a setup that chattered on aluminium will fail here. We run carbide with heavy coolant and conservative radial engagement. If a feature can be designed in aluminium instead, the part gets cheaper and faster.

Stainless 17-4PH (SUS630) and 316L cover most of the corrosion-resistant hardware we see. 17-4PH machines reasonably in the annealed condition and gains strength after aging; 316L galls easily and needs sharp tools and steady feed. Inconel is the hardest case. It work-hardens under a rubbing cut, so we take a real depth of cut and never dwell.

Plastics and composites appear in non-structural panels and ducts. PEEK and POM machine to tight tolerance with sharp cutters and air blast. Carbon fibre is abrasive; it dulls carbide quickly and the dust needs extraction. For those parts, consider whether the geometry is better served by another process before you commit to cutting.

Cutting is not always the answer. A part with a wall thinner than about 0.5 mm on a long span will deflect under cutting force, and no amount of care fixes that. A thin-wall duct is usually better formed or printed. A part with internal channels that cannot be reached by a tool is a candidate for additive work.

Very high quantities also change the math. At one to a few hundred pieces, milling and turning are competitive because there is no tooling cost. At 10,000 pieces and up, a cast or forged blank with a light finish cut often lands cheaper, and it gives you better grain structure for a structural part. We will say so if that is the case.

Material utilization is another factor. A large plate part cut from solid can leave more than half the stock as chips. If the geometry allows, a near-net forging or a weldment reduces both cost and lead time. For prototypes, cutting from solid is almost always the fastest path to a real part in your hands.

There are also features we simply cannot cut. Sharp internal corners cannot be produced by a round tool; the corner radius is the tool radius. Undercuts need a fifth axis or a special cutter. Deep holes past roughly ten times diameter need gun drilling or EDM. Bring these up at quote time, not after the first article.