What Parts Are Generally Processed by CNC Machining

• 1
  Key takeaways
• 2
  Parts Processed by CNC Machining: Box-Type Bodies
• 3
  Special-Shaped Parts With Asymmetric Features
• 4
  Discs, Sleeves and Plate Parts: Rotation and Flatness
• 5
  Contoured and Freeform Surfaces
• 6
  Thin-Wall and Micro Parts: Where Rigidity Runs Out
• 7
  Which Group Fits Which Machine

Box-type parts are the workhorse of milling. Think gearbox housings, pump bodies, valve blocks, and engine blocks. The shape is mostly prismatic: flat faces on several sides, bored holes through those faces, and pockets or slots between them. What makes the group distinct is that hole positions and face parallelism matter more than the outer contour. A gearbox housing with bearing bores 0.02 mm off will whine, even if the casting looks perfect.

A three-axis mill handles a box part when all machined faces are reachable from five or six setups. That is the classic approach and still the cheapest. Add a fourth axis or a Ø400 mm rotary table and you cut the setups in half, because the part indexes instead of being re-clamped. On our 16 simultaneous 5-axis centers, a housing with bores on four sides often runs in two setups instead of six.

The engineering trade-off is stiffness. A box part with thin ribs and large openings can deflect under clamping force. We usually recommend leaving stock on the outer walls until the bores are finished, then taking a light pass at Ra 1.6–3.2 μm to relieve stress. If the wall is under 2 mm, plan on a support fixture or a low-melting-point filler.

Materials for box parts are typically cast aluminium ADC12, 6061-T6 plate, or cast iron. Castings need one more check: the first cut tells you whether the casting shifted, and that decides whether you machine to nominal or to an offset datumed off the bore.

Special-shaped parts are the ones that do not fit a box. Brackets with compound angles. Arms with offset bosses. Housings with a curved boss sitting at 37° to the main face. The geometry is asymmetric, so there is no single obvious datum, and the first question in a DFM review is always where the tolerance stack starts.

These parts are where 5-axis earns its cost. A compound-angle face that would need a custom angle plate on a 3-axis machine becomes a single indexed cut. On a simultaneous 5-axis center the tool stays normal to the surface, which keeps the effective cutter diameter constant and avoids the scallop you get when a ball nose runs at a shallow angle.

The risk with special-shaped parts is over-tolerancing. Teams often copy a ±0.005 mm callout onto every dimension because the drawing looks complex. In practice, only two or three features usually control function: a bore, a mounting face, a pin location. Mark those and let the rest sit at ±0.1 mm. That single decision often removes a finishing operation.

For prototypes, rapid prototyping on the same machines keeps the geometry honest. A low-volume run of 20 special-shaped brackets can start within 24 hours and ship in 3–5 days, with the same program used later for the production batch.

Discs, sleeves and plates are turned parts first and milled parts second. A disc is mostly a diameter with a thickness: flanges, brake rotors, bearing covers, impellers. A sleeve is a diameter with a bore through it: bushings, spacers, hydraulic cylinders. A plate is a thickness with a perimeter: manifold plates, cover plates, base plates.

Sleeves and discs go on a lathe or a mill-turn center. Concentricity between the OD and the ID is the controlling tolerance, and it is set by how the part is held. Turning between centers holds concentricity well. Chucking on a thin sleeve distorts it, so we often rough, release, then finish with light passes at Ra 0.8–1.6 μm.

Plates look simple and are not. A 6 mm aluminium plate 300 mm long will bow when you face it, because the rolled stock has internal stress. The fix is to face both sides in alternating light passes, or to stress-relieve the plate first. If flatness matters more than thickness, say so on the drawing; the machining sequence changes.

Mill-turn centers are the practical answer for parts that are round and prismatic at once, such as a shaft with a milled flat and cross-drilled hole. One machine, one setup, one datum. That removes the concentricity error you get when the part moves from lathe to mill.

Contoured parts have no flat face to reference. Turbine blades, impellers, medical instrument handles, aerodynamic housings, mould inserts. The surface is defined by a CAD model, and the CAM toolpath is what turns that model into metal. There is no drawing dimension for most of the surface, only a profile tolerance.

Cutting these parts is a question of tool access and stepover. A ball nose cutter at 0.2 mm stepover on a 50 mm surface gives a finish around Ra 0.8–1.6 μm and takes time. Tightening the stepover to 0.1 mm roughly doubles the cycle. If the surface is cosmetic only, a coarser pass plus bead blasting or polishing reaches the same look for less money.

Five-axis simultaneous motion is what keeps the tool normal to a compound curve. On a 3-axis machine, a steep wall forces the cutter into a shallow engagement, which raises radial force and chatter. We reserve the 16 simultaneous 5-axis centers for exactly this geometry.

Undercuts are the hard limit. If a feature cannot be reached by any tool axis without colliding with the part, milling stops there. Options are a longer reach tool with a smaller shank, which deflects, or splitting the part into two pieces and joining them.

Thin-wall parts are defined by their ratio, not their size. A wall under 1 mm on a 50 mm aluminium part, or under 0.5 mm on a small stainless part, behaves like a spring. Clamping force moves it, cutting force vibrates it, and the finished part relaxes when you unclamp it.

The standard countermeasures are low clamping pressure, sacrificial tabs that hold the wall until the last operation, and light finishing passes. For a 0.8 mm aluminium wall we typically leave 0.3 mm of stock, run a semi-finish, then take two 0.15 mm passes at high spindle speed. High speed reduces the cutting force per tooth, which is what actually causes the wall to deflect.

Micro parts, meaning features under 1 mm, need small tools and clean coolant. A 0.5 mm end mill has very little stiffness, so depth of cut stays shallow and the feed per tooth drops. Tool breakage, not tolerance, is the main cost driver here.

If a part is thin-walled and also needs a tight flatness callout, say so early. Flatness on a flexible part is measured in the free state, and the fixture has to be designed so the part is not held flat by force.