Precision CNC machining of aerospace parts

• 1
  Key takeaways
• 2
  Where the tolerance budget actually goes
• 3
  Why five-axis setups hold aerospace features
• 4
  Material behaviour on aerospace parts
• 5
  Thin walls, chatter, and the real accuracy ceiling
• 6
  Inspection, datums, and what the report means
• 7
  From RFQ to shipped aerospace parts
• 8
  Which setup suits which aerospace feature

A drawing that reads ±0.005 mm everywhere is not a strict drawing. It is an unfinished one. On a machined aerospace part, that number is a budget you spend across the whole process chain: raw stock condition, fixture rigidity, thermal drift, tool wear, and the CMM that measures the result.

Start with the datum. If the primary datum is a rough casting face, everything downstream inherits its flatness error. The fix is to establish a machined datum in the first operation, then reference every later cut to that face. We call this a process datum, and it is usually what makes a tight tolerance repeatable rather than lucky.

Thermal drift is the quiet cost. Aluminium 7075 expands about 23 μm per meter per °C. A 300 mm bracket that warms 4 °C between roughing and finishing moves roughly 28 μm. That is already more than the tolerance you asked for. Rough, let the part rest, then finish.

Tool wear adds a slow bias. A carbide end mill cutting 7075 loses a few micrometres of edge radius over a long run, and the last 20 parts in a batch can drift outside the band that the first 20 held. We change tools on a count, not on a hunch.

• 1
  Rough and finish in separate operationsRemoves residual stress and lets the part reach room temperature.
• 2
  One datum, used everywhereMachined in op 1, referenced by every fixture after that.
• 3
  Measure at 20 °CA part measured hot will fail inspection later in the customer's lab.

The value of simultaneous 5-axis machining is not that it reaches strange angles. It is that it removes re-fixturing. A typical engine bracket with pockets on three faces needs six setups on a 3-axis mill and two on a 5-axis center. Each setup you delete removes a stack of positional error that no tolerance callout can recover.

Short tools matter just as much. Tilting the part lets a stub end mill reach a deep pocket wall without a long, flexible cutter. A 12 mm diameter tool hanging 60 mm out of the holder deflects under load; the same tool held at 30 mm out cuts a straighter wall, and the surface finish improves without any change to feed or speed.

Contouring in five axes also keeps the tool normal to a curved surface. That gives an even scallop height across a blade root or a duct flange instead of the banding you get from a ball nose running at a fixed angle. On Ra 0.8–1.6 μm work, that difference shows up on the first article.

There is a limit. Five-axis setups are slower to program and slower to prove out. For a flat plate with holes on one face, a three-axis machine with a good fixture will beat it on cost and often on lead time.

• 1
  Good fitPockets on multiple faces, contoured surfaces, deep cavities needing short tools.
• 2
  Poor fitSimple prismatic parts, single-face work, very small batches of loose-tolerance items.

Aluminium 7075 machines cleanly and holds a good finish, but it is notch sensitive and stresses relieve when you remove material. A part that is straight off the machine can bow overnight if the stock was not stress-relieved. 6061-T6 is more forgiving and is often the better choice for housings and brackets where strength is not the governing load case.

Titanium Ti-6Al-4V is where the process changes character. It conducts heat poorly, so the cutting edge takes the temperature. Speeds drop to roughly a third of what aluminium allows, coolant must reach the edge, and tool life becomes a planning item rather than a surprise. A titanium part quoted at aluminium cycle times is a quote that will be revised.

Inconel and the nickel alloys push further. They work-harden at the surface, so a cutter that rubs instead of cutting will harden the next pass. We keep radial engagement light and never let the tool dwell in the cut. These parts need more time and more inspection, and the cost reflects that.

Stainless 17-4PH sits in the middle. It holds tolerance well, machines predictably in the H1025 condition, and takes a good electroless nickel or passivation finish. For brackets and fittings, it is often the compromise that satisfies both the stress engineer and the shop.

• 1
  7075Strong, machines well, but relieve stress or expect movement.
• 2
  Ti-6Al-4VSlow speeds, high heat at the edge, plan for tool wear.
• 3
  InconelLight radial engagement, no dwelling, more inspection.
• 4
  17-4PHPredictable, good for fittings and hardware.

The accuracy limit on most aerospace parts is not the machine. It is the stiffness of the part itself. A 0.8 mm wall in aluminium has almost no resistance to a side load. Push a normal radial depth of cut and the wall deflects away from the tool, then springs back and takes a heavier cut on the next tooth. You hear it before you measure it.

The practical fix is to stop trying to remove material in one pass. Light radial engagement, high spindle speed, and a smaller step-down keep the cutting force low enough that the wall stays where it is. A 6 mm end mill taking 0.5 mm radial and 2 mm axial at high rpm will hold a wall that a heavy pass would destroy.

Support helps too. Wax, low-melt fixturing compound, or a machined temporary web can hold a thin section until the last operation. The web is then cut away in a finishing pass. It costs programming time and it saves the part.

Chatter shows up as a pattern on the surface and as a wandering dimension. If a finish cut sounds different on the second pass than the first, stop and check the setup. Changing speed often fixes it faster than changing the tool.

• 1
  Reduce radial engagement firstRadial depth affects force more than axial depth does.
• 2
  Add temporary supportWax or a machined web until the final pass.
• 3
  Listen to the cutA tone change between passes means the setup moved.

Inspection is part of the process, not a step at the end. If a feature is not measured, it is not controlled, no matter what the drawing says. We agree the datum scheme with the customer before the first cut on any tight-tolerance part, because a CMM report that uses different datums than the drawing is a report nobody can accept.

For a typical bracket, that means a CMM program aligned to the three datum planes on the drawing, with the critical bores and faces evaluated against them. For a turned part, roundness and coaxiality get checked on a roundness tester, not just a caliper. Bores at ±0.005 mm are reamed or bored, not drilled, and then measured with a bore gauge that reads to 1 μm.

Surface finish is measured, not eyeballed. Ra 0.2–0.8 μm is a fine finish and requires a controlled finishing pass. Ra 1.6–3.2 μm is as-machined and looks fine for non-sealing faces. Ask for the finish you need on the face that needs it, and leave the rest alone. Every extra fine surface adds cycle time.

Every part we ship is inspected before it leaves. Raw material certificates are checked on receipt, in-process dimensions are monitored during the run, and the final inspection report is available on request. For aerospace buyers, that paper trail is often as important as the part.

• 1
  Agree datums before cuttingA report on different datums cannot be accepted.
• 2
  Fine finish only where neededSealing faces, bearing bores, and sliding surfaces.
• 3
  Paper trailMaterial certs and final inspection reports on request.