CNC milling fundamentals

• 1
  How a milling cutter actually removes material
• 2
  What the axes really control: 3-axis vs 4-axis vs 5-axis
• 3
  Roughing, finishing and the tool path in between
• 4
  Which materials mill well, and which fight back
• 5
  What ±0.005 mm does and does not mean
• 6
  Which milling setup fits the part

Milling is subtractive. A multi-flute cutter spins on a spindle and is fed sideways into a solid block, so each tooth takes a small chip and the part is left behind. The workpiece is usually clamped still while the tool moves in X, Y and Z. That is the opposite of turning, where the part spins and a single-point tool feeds along it.

The chip has to leave the cut. If it stays in the flute, it gets re-cut, heats up, and welds to the edge. Flute count, helix angle and coolant all exist to move chips out of the way. A three-flute cutter in aluminium cuts fast and clears well. A four- or five-flute cutter in steel produces a thinner chip per tooth but leaves a better floor finish.

Heat is the real limit. The tool edge, the chip and the part all rise in temperature at the contact zone. Too much heat softens the edge and pushes material around instead of shearing it. That shows up as a shiny, smeared wall and a short tool life.

The practical setting is surface speed and feed per tooth. In 6061 aluminium, cutting speeds often run 300–500 m/min. In 17-4PH stainless, they drop to 60–120 m/min. The cutter does not care what the drawing says. It cares about the material in front of it.

• 1
  Climb millingTooth enters at full chip thickness; standard for CNC with low backlash.
• 2
  Conventional millingTooth rubs before it cuts; used on older manual machines.
• 3
  Depth of cutRadial 30–50% of cutter Ø is a common roughing start.

A 3-axis mill moves the tool in X, Y and Z only. Every feature has to be reachable from the top, or the part gets re-fixtured and re-datumed. Each new setup adds a small position error, and that error stacks. Three-axis work is still the cheapest way to cut a flat plate with pockets and holes.

Adding a rotary table gives the fourth axis, usually rotation about X. Now the part can be indexed to several faces without being unclamped. This suits shafts with cross-holes, or a part with features on four sides that all reference one bore. Indexing is not the same as continuous motion, though. The table moves, stops, locks, then cuts.

Five-axis means the tool and the workpiece can move and rotate together. Simultaneous five-axis lets a short, stiff cutter tilt into a deep pocket instead of hanging out of the holder. It also reaches undercuts and blended surfaces in one setup.

The trade is programming time and machine cost. Simple prismatic parts rarely justify it. Parts with compound angles, deep cavities, or tight true-position callouts across several faces usually do.

• 1
  3-axisFlat plates, pockets, through-holes, one accessible direction.
• 2
  4-axisCylindrical parts and indexed faces around one axis.
• 3
  5-axisCompound angles, undercuts, blended surfaces, one setup.

Roughing removes the bulk of the stock and leaves a uniform allowance for finishing, typically 0.2–0.5 mm on walls and floors. A trochoidal or high-efficiency path keeps the radial engagement low and the axial depth high, which spreads wear along the flute instead of burning one spot.

Finishing decides the surface and the final size. A ball-nose cutter leaves scallops, and the stepover sets how tall they are. Halving the stepover roughly quarters the scallop height. That is why a smooth curved surface takes far longer than a flat one at the same tolerance.

Thin walls are the classic trap. As the wall gets below about 1 mm, cutting force pushes it away from the cutter, the tool rubs, and the wall comes out tapered or chatters. Light passes and support on both sides help. Sometimes the honest answer is to leave more material and machine it in a second operation.

Tool reach matters as much as tool diameter. A cutter hanging 4× its diameter out of the holder deflects. Keep the gauge length as short as the geometry allows, and use a necked cutter to reach a deep pocket rather than a long, skinny one.

• 1
  Allowance0.2–0.5 mm left after roughing for finishing passes.
• 2
  StepoverSmaller stepover gives a shorter scallop, not a tighter tolerance.
• 3
  Wall thicknessBelow ~1 mm, expect deflection and chatter without support.

Aluminium is the easy case. 6061-T6 and 7075 cut fast, hold a good finish and take fine threads without much trouble. 6061 is the default for fixtures and housings. 7075 gives higher strength but is less forgiving of a dull edge.

Stainless moves the problem. Grades 303 and 304 work-harden if the cutter rubs instead of cutting, so a light pass with a dull tool makes the next pass harder. 316L is common in medical and food parts. 17-4PH can be machined in the solution-treated condition and then aged, but the aged condition is slow going.

Titanium and nickel alloys are where the process slows down. Ti-6Al-4V conducts heat poorly, so the edge takes almost all of it. Inconel is worse. Both need sharp tools, low surface speed, generous coolant and a rigid setup.

Plastics behave differently again. POM and PEEK machine cleanly with sharp, polished flutes and high spindle speed. ABS and PC soften with heat and can gum up. The main risk is melting, not chipping.

• 1
  Aluminium6061-T6, 7075, 6082; fast, clean, good for prototypes.
• 2
  Stainless303, 304, 316L, 17-4PH; avoid rubbing and work hardening.
• 3
  Titanium and InconelLow speed, sharp edge, rigid setup, heavy coolant.
• 4
  PlasticsPOM, PEEK, PA cut clean; ABS and PC need sharp flutes.

A stated tolerance is a capability, not a promise on every feature. ±0.005 mm is achievable on a ground or bored feature in a rigid setup, measured at a controlled temperature. It is not achievable on the far end of a thin, unsupported wall.

Temperature is part of the number. Aluminium expands about 23 μm per metre per °C. A 100 mm part measured 5 °C off from the machining temperature has already moved roughly 12 μm. That is more than the tolerance band.

Surface finish and tolerance are separate costs. A tight bore and a fine finish often come from different operations. A reamed or bored hole can be precise while still being rough. A polished surface can be smooth while being loose.

So the useful question is not what tolerance a shop can hold. It is which features actually need the tight number, and which can live at ±0.1 mm. Marking only the critical ones keeps the part affordable.

• 1
  Critical featuresDatums, bearing bores, mating faces; call these tight.
• 2
  Free featuresClearance holes, edges, non-mating faces; leave at ±0.1 mm.
• 3
  MeasurementAsk how a tight feature is verified, not just cut.