Overview of CNC Milling Parts

• 1
  Overview of CNC milling parts: how a cutter removes metal
• 2
  Which features need 3, 4 or 5 axes
• 3
  Where tolerance and surface finish come from
• 4
  Material choice changes the cut, not just the part
• 5
  Choosing the right setup for a milled part

Milling is subtractive. A multi-flute cutter rotates at 3,000 to 20,000 rpm and is fed sideways through a solid block. Each tooth catches a chip of material and throws it clear. The shape you get is whatever space the cutter's swept volume leaves behind. That is the whole idea, and it sets the limits of the process.

Three numbers control the cut. Surface speed decides how fast the edge travels past the material. Feed per tooth decides how thick each chip is. Depth of cut decides how much engagement the flutes see at once. Push any one too hard and the tool deflects or chips. Push all three too gently and the cutter rubs instead of cutting, which burns the edge and work-hardens stainless.

Rigidity matters more than spindle power on small parts. A 6 mm end mill hanging 40 mm out of the holder will chatter long before the spindle runs out of torque. Shorten the gauge length or step up to a 10 mm cutter and the same cut runs quiet. That is why tool reach, not machine size, often sets the floor on feature size.

The cutter never leaves a sharp internal corner. A pocket milled with a Ø10 mm tool carries a 5 mm corner radius at minimum. Designers who draw a true 90° internal corner force the shop into EDM or a drilled relief. Add the radius in CAD and the part stays a milling part.

• 1
  Climb millingTooth enters at maximum chip thickness. Better finish, less rubbing, standard on CNC.
• 2
  Conventional millingRarely used now. Mostly for rough castings with hard surface scale.
• 3
  Chip evacuationDeep pockets need air blast or through-coolant. Recut chips kill the edge.

A 3-axis mill moves X, Y and Z. The tool always points down. This covers most prismatic parts: plates, brackets, housings with pockets on one face, and anything you can reach from six orthogonal directions. If the part can be re-fixtured and re-datumed for each face, 3-axis work is the cheapest route. It is also the most repeatable, because each setup is simple.

A 4-axis mill adds a rotary table, usually Ø400 mm, turning about X. Now the part rotates under the cutter. This suits shafts with flats, cylinders with cross-drilled holes, and parts with features wrapped around an axis. One setup replaces three or four. Fewer setups mean less datum stack-up, and that shows up as tighter true position between features.

A 5-axis mill adds a second rotary axis. The tool can tilt, so it approaches a face at an angle instead of straight down. That does two things. It reaches undercuts and deep cavities that 3-axis cannot touch, and it lets a stubby cutter follow a contoured surface, which raises rigidity and improves finish on sculpted geometry. Impellers, turbine blades and medical implants are the classic cases.

Five axes is not automatically better. Simultaneous 5-axis motion costs more per hour and needs more programming time. For a flat bracket with holes on four sides, 3-axis with two setups beats it on price and on lead time. Use 5-axis when the geometry is unreachable, when one setup is worth more than the machine rate, or when a contoured surface needs a short, stiff tool.

• 1
  3-axisPrismatic parts, six-sided access, tight budget, high repetition.
• 2
  4-axisRotational parts, wrapped features, fewer setups, better feature-to-feature position.
• 3
  5-axisUndercuts, deep cavities, contoured surfaces, single-setup accuracy.

Tolerance is not a single number for the whole part. It is a budget you spend feature by feature. On a well-set-up machine we hold ±0.005 mm (±0.0002 in) on critical dimensions, but applying that to every hole and face drives cost up with no benefit. Mark the two or three features that mate with something else. Leave the rest at general tolerance and the part gets cheaper without losing function.

Surface finish is set by the last pass, not by the whole program. As-machined surfaces land at Ra 1.6–3.2 μm. A finishing pass with a smaller stepover and a sharp insert reaches Ra 0.8–1.6 μm. Polishing or fine boring on a specific face can reach Ra 0.2–0.8 μm. Rough the part fast, then slow down only where the drawing calls for it.

Thermal drift fights you on tight work. Aluminium expands about 23 μm per meter per °C. A 300 mm part that warms 5 °C during roughing grows 0.035 mm, which is seven times the tolerance band. Good shops rough, let the part cool, then finish. They also measure at 20 °C. If your drawing says ±0.005 mm, that is measured cold, not straight off the machine.

Thin walls move too. A 0.8 mm aluminium wall will deflect away from the cutter under radial load. Expect to leave stock, come back with a light spring pass, and accept that walls under 0.5 mm need support or a different process. Milling is forgiving on many things. It is not forgiving on unsupported thin sections.

• 1
  General toleranceNon-critical faces and holes. Keeps the quote down.
• 2
  Critical toleranceBearing bores, mating faces, dowel holes. Spend the budget here.
• 3
  Inspection100% before shipment. Reports available on request.

Aluminium 6061-T6 is the default for milled parts. It cuts fast, holds tolerance well, and anodizes cleanly. 7075 gives higher strength but is notch-sensitive and machines with a gummier chip. 2024 has better fatigue life and worse corrosion resistance, so it usually needs a coating. For housings and covers, 5052 and 6082 both machine well and weld easily.

Stainless is where feeds and speeds matter most. 303 is free-machining and the easiest of the family. 304 and 316 work-harden if the cutter rubs, so you keep the feed up and take a real chip. 17-4PH gives high strength after aging, and it holds a good finish on medical and aerospace parts. 316L is the pick where corrosion resistance outranks strength.

Titanium Ti-6Al-4V (TC4) cuts at roughly a quarter of the speed of aluminium and pulls heat into the tool rather than the chip. Tool life drops, so does metal removal rate. It is still milled every day for aerospace brackets and medical hardware. Budget more time and use plenty of coolant. Inconel is harder again and often needs ceramic or carbide tooling run at low surface speed.

Plastics mill cleanly if you manage heat. POM and PEEK hold tolerance well. ABS and PC can melt and smear at the edge, so you run sharp tools, high rake, and air blast instead of flood coolant. Carbon fibre is abrasive and eats carbide, so you plan on more tool changes. The material you pick changes cycle time, tooling and finish, not just the part.

• 1
  Fast and easy6061, 6082, 303 stainless, POM.
• 2
  Strong but slower7075, 17-4PH, 4140, Ti-6Al-4V.
• 3
  Hard on toolsInconel, carbon fibre, beryllium copper.