CNC Cutting Processing: How Metal Removal Actually Works

• 1
  What CNC cutting processing removes, and why it is controlled
• 2
  Milling, turning, EDM, laser and waterjet: what each cut gives you
• 3
  Where CNC cutting processing hits its limits
• 4
  Tolerance, finish and inspection in real production
• 5
  Material behaviour changes the cutting plan
• 6
  Which cutting process fits which job

Cutting is the oldest idea in metalworking and the least forgiving. A tool edge is forced into material that will not move out of the way on its own, so the material ahead of the edge deforms, fractures, and slides up the rake face as a chip. Every number a programmer sets — feed per tooth, spindle speed, depth of cut — is really a statement about how that chip forms. Get the chip wrong and the tool rubs, work-hardens the surface, or breaks.

CNC cutting processing replaces the hand on the wheel with a controller reading a program. On a milling center the workpiece is clamped and the spindle moves in X, Y and Z while the tool spins. On a lathe the part turns and a single-point tool feeds along the axis. Both cases follow the same rule: the tool path is fixed by code, so the cut repeats exactly on part two and part two thousand.

The chip carries the heat away. That is the part most people miss. When the chip is thick enough, most of the cutting energy leaves with it, and the part stays cool. When the chip is thin — a light finishing pass with a worn edge — the energy stays in the workpiece, and you get a shiny surface with a hard, stressed layer under it. That layer shows up later as distortion after anodizing or as a cracked thread root.

The controller only knows position, not condition. It cannot feel a dull insert or a chip packed in a pocket. That is why cutting parameters are written for the material and the tool, not for the machine alone. Aluminium 6061 at 3,000 rpm and Inconel at the same speed are not the same operation. One cuts clean, the other destroys the edge in under a minute.

• 1
  Chip thickness drives heatToo thin and the energy stays in the part
• 2
  Tool path is repeatableThe program, not the operator, sets the geometry
• 3
  Parameters belong to the material pairWorkpiece plus tool grade decides speed and feed

Milling covers the widest range. A rotating multi-tooth cutter removes material in passes, so pockets, slots, faces, and contoured walls all come off the same setup on a 3-axis machine. Add two rotary axes and you reach undercuts and angled faces without re-fixturing, which is where the tolerance stack stops growing. Our 16 simultaneous 5-axis centers hold ±0.005 mm on features that would need four setups otherwise.

Turning is for parts that are round and mostly symmetrical. A single-point tool follows the profile as the part rotates, and the geometry is generated by the tool nose radius. That is why a turned surface carries a spiral lay and why a shoulder needs a relief groove — the tool cannot cut a square internal corner. Mill-turn centers combine both motions, so a shaft with cross-drilled holes and a milled flat comes off one machine.

Thermal cutting works differently. Laser and plasma melt or vaporize the material, and waterjet erodes it with abrasive. None of them touch the part with an edge, so hardness stops mattering. The trade is edge quality and thickness. Waterjet cuts 100 mm stainless with a square edge and no heat-affected zone, but it is slow and the taper grows with thickness. Laser is fast on 1–6 mm sheet with a fine kerf, yet the cut edge is a heat-affected zone that may need a secondary pass.

EDM removes material with sparks between an electrode and the work, submerged in dielectric fluid. It cuts any conductive material regardless of hardness, which makes it the answer for hardened tool steel and sharp internal corners. It is slow and needs an electrode, so it rarely competes with milling on open geometry. Use it where the corner radius is smaller than any end mill could reach.

The rule is simple. If a rotating cutter can reach the feature, mill or turn it. If it cannot, or the material is already hardened, go thermal or EDM. Mixing methods on one part is normal; a hardened die insert is often milled soft, heat treated, then wire-cut and EDM-finished.

• 1
  Milling and turningBest cost per feature on open geometry
• 2
  Laser and plasmaSheet and plate, fast, heat-affected edge
• 3
  WaterjetThick plate, no heat, slower and tapered
• 4
  EDMHardened material, sharp internal corners

Cutting cannot make a feature smaller than the tool that reaches it. A 3 mm internal corner needs a 3 mm cutter, and that cutter is short and slow. Deep pockets with small radii are where cycle time and cost jump. If the design allows a 6 mm corner radius instead of 3 mm, the same pocket can be cut with a tool four times stiffer, and the surface finish improves with it.

Wall thickness matters as much as feature size. A 0.5 mm aluminium wall will deflect under cutting force and chatter, even with a light pass. The part may measure correctly on the machine and spring back after unclamping. For thin walls, we rough with stock left on, stress-relieve or rest the part, then take a finishing pass with low radial engagement.

Hardness sets a ceiling. Above roughly 45 HRC, carbide edges wear fast and the cut becomes unpredictable. Pre-hardened steels in the 30–40 HRC range cut well with the right grade. Above that, the part is normally machined soft and hardened afterward, or the hard features are finished by EDM and grinding.

Aspect ratio decides whether the cut is stable. A tool that is eight times longer than its diameter will chatter at almost any speed. Deep cavities and tall ribs push you into long, thin tools, and the fix is usually a design change or a different process, not a faster spindle.

Cutting also leaves marks. Tool marks, cutter sweep lines, and witness lines from a previous setup are all normal on an as-machined surface at Ra 1.6–3.2 μm. If the drawing calls for Ra 0.2–0.8 μm, plan a finishing operation or a secondary process such as bead blasting or polishing. Surface callouts and tolerance callouts should be decided together, because a tight finish on a loose dimension wastes money.

• 1
  Internal cornersLimited by the smallest rigid cutter
• 2
  Thin wallsDeflect and spring back after unclamping
• 3
  Hardness above 45 HRCPlan soft machining plus EDM or grinding
• 4
  Long toolsChatter long before they break

A tolerance is a statement about the whole chain, not just the machine. Fixture rigidity, thermal drift, tool wear, and the measurement method all sit inside that number. A ±0.005 mm callout on a 300 mm aluminium plate is achievable, but it needs a temperature-stable shop floor and a CMM check, not a caliper reading taken at the machine.

Tool wear is the slow variable. A carbide insert that starts sharp will hold size for a while, then drift as the edge rounds. On long runs we track the offset and compensate before the feature leaves tolerance, rather than inspecting every part and scrapping the ones that drifted. That is how a 99.99% qualification rate is held across a production run.

Finish is set by the last pass, not the whole program. Feed per tooth, tool nose radius, and cutting speed determine the cusp height between passes. To reach Ra 0.2–0.8 μm on aluminium, you need a sharp tool, a small stepover, and a speed high enough to avoid built-up edge. On stainless 316L the same target needs a different grade and a slower surface speed, because the material work-hardens.

Inspection proves the result. We check raw material certificates on receipt, monitor dimensions in process, and inspect 100% of parts before shipment, with reports available on request. For medical and automotive work, the inspection plan follows ISO 13485:2016 and IATF 16949:2016 requirements, so traceability is documented at every step.

Setup count is the hidden cost. Every new orientation adds a fixture, an alignment step, and a chance for stack-up error. A part that needs five setups can usually be redesigned or re-fixtured to need two. Fewer setups means tighter true position and a shorter lead time, not just a cheaper part.

• 1
  Tolerance includes the setupFixture, drift and gauge all count
• 2
  Compensate for wearAdjust offsets before parts drift out
• 3
  Finish follows the last passStepover and nose radius set the cusp
• 4
  Document everythingMaterial certs and inspection reports on request

Aluminium 6061 cuts freely and holds a good finish at high speed. It is the default for prototypes and enclosures, and it machines at rates that make short runs economical. The 7075 grade is stronger but more brittle, and it needs sharper tools and better chip evacuation or the edges chip.

Stainless behaves differently. Grades 303 and 304 gummy, 316L worse. The material work-hardens under the edge, so a light rubbing pass makes the next pass harder. The fix is a positive rake, a firm feed per tooth, and never letting the tool dwell. Coolant matters more here than on aluminium.

Titanium TC4 (Ti-6Al-4V) and Inconel sit at the hard end. Both hold heat in the cut and both destroy edges quickly. Speeds drop by a factor of five or more compared with aluminium, and tool life is measured in minutes, not hours. These materials need a rigid setup and a conservative approach, so quote them with the right cycle time rather than the optimistic one.

Plastics and composites follow their own rules. POM and PEEK cut clean with sharp, polished flutes and high speed, but they melt if the chip cannot clear. Carbon fibre needs diamond-coated tooling because the fibres abrade carbide fast. Climb milling helps on all of them, since it keeps the cut on the thick side of the chip.

• 1
  Aluminium 6061Fast, predictable, good default
• 2
  Stainless 316LWork-hardens, needs firm feed
• 3
  Titanium and InconelSlow speeds, short tool life
• 4
  Plastics and CFRPSharp flutes, high speed, good chip clearance