CNC cutting: how each process removes material, and where it stops

• 1
  What CNC cutting actually does to metal
• 2
  Tolerance, finish, and the cost of holding them
• 3
  Why the setup decides the outcome more than the spindle
• 4
  Material behavior at the cut
• 5
  Which CNC cutting process fits which feature

Every CNC cutting operation does one of three things at the tool tip: it shears material off with a hardened edge, it melts and blows material away with a focused beam, or it erodes material with a spark. Milling, turning, and drilling are the first kind. Laser is thermal, waterjet is mechanical erosion, and wire EDM works by spark. The physics of that single interaction sets the tolerance, the surface finish, and the heat-affected zone you will live with.

Shearing cuts use a defined cutting edge, so the geometry of the tool decides what features you can reach. A 6 mm end mill with 3× flute length can only reach 18 mm deep before the shank rubs the wall. Deep pockets and internal corners therefore need either a long-reach tool, which deflects, or a different process entirely. This is why a part with a 40 mm deep, 8 mm wide slot is a poor milling candidate but a routine wire EDM job.

Thermal cuts ignore tool stiffness. A laser or plasma head never touches the part, so depth is not limited by reach. What limits them is heat. A 3 mm stainless sheet cut by fiber laser will show a narrow heat-affected zone and slight taper on the kerf, typically 0.1–0.2 mm wide. Thicker sections need more power, and the edge quality drops as the beam spreads through the material.

Erosion cuts remove material atom by atom with electrical discharge. Because there is no mechanical force, wire EDM can cut hardened tool steel at 60 HRC without distortion, holding ±0.005 mm. The trade-off is speed and conductivity. The workpiece must conduct, and a 100 mm thick cut runs slowly. For a hardened punch die with a sharp corner, that slowness is usually worth it.

• 1
  ShearMilling, turning, drilling: fast, tool geometry limited
• 2
  ThermalLaser, plasma: no contact, heat-affected edge
• 3
  ErosionWire EDM: hard materials, slow, needs conductivity

Tolerance on a CNC cutting job is not one number for the whole part. It is a stack of contributions: machine positioning, tool deflection, thermal growth, and fixturing repeatability. A modern 5-axis center positions to a few microns, but a long end mill in a deep pocket can deflect 0.05 mm under load. That deflection, not the machine spec, usually decides whether you hit ±0.005 mm.

Surface finish is a separate bill. A sharp tool at the right feed leaves Ra 1.6–3.2 μm as-machined, which is fine for most brackets. Push to Ra 0.8–1.6 μm and you need lighter passes, sharper inserts, and often a finishing toolpath that adds cycle time. Below Ra 0.8 μm, you are usually polishing or lapping after the cut, not cutting to that finish directly.

Hardness matters here. Aluminium 6061 cuts cleanly at high speed and holds tight tolerance without much fuss. Stainless 316 work-hardens if the feed is too light, so the same tolerance requires a more rigid setup and a heavier chip load. Titanium Ti-6Al-4V adds heat to the tool edge, so tool life drops and the finish drifts unless coolant and speed are dialed in.

The practical answer is to tolerance only what functions. If a bore locates a bearing, hold it. If a clearance hole passes a bolt, ±0.1 mm is plenty and it costs less. Over-tolerancing a whole drawing is the most common way a simple CNC cutting job becomes expensive.

• 1
  ±0.005 mmAchievable, but deflection and fixturing decide it
• 2
  Ra 0.8–1.6 μmStandard fine finish, adds cycle time
• 3
  Below Ra 0.8 μmUsually a polishing step, not a cutting step

A rigid machine with a weak fixture cuts like a weak machine. When a part moves 0.02 mm under cutting load, no amount of spindle accuracy recovers it. Good CNC cutting starts with workholding: vise jaws machined to the part, soft jaws for thin walls, or a vacuum plate for flat sheet. For a 1 mm wall, the clamping force alone can bow the part before the tool touches it.

Thin-wall parts need support on both sides. One common approach is to leave a sacrificial web, cut the profile, then remove the web in a second operation. Another is to fill the pocket with a low-melt wax or fixturing compound, cut, then melt it out. Both add a step. Both keep the wall straight.

For a first article, we check the setup before the geometry. Measure the datum, confirm the part sits flat, and cut a test feature. If the datum moves, the whole tolerance stack is wrong. Our inspection covers raw material, in-process checks, and a final check before shipment, with reports on request.

Five-axis work changes the fixturing question. A part that needs four sides can often be cut in one setup on a 5-axis center, which removes three re-clamping errors. That is the real gain: fewer setups, not just more angles. We run 16 simultaneous 5-axis centers for exactly this reason.

• 1
  Soft jawsMachined to the part, spreads clamping force
• 2
  Sacrificial webHold thin walls, remove in a second op
• 3
  One setup5-axis cuts four sides without re-clamping

Aluminium is the easy case. Grades 6061, 7075, and 6082 cut fast, hold ±0.005 mm without drama, and take a fine finish. The catch is 7075: it is stronger but more prone to stress movement after heavy material removal, so rough, stress-relieve, then finish. For a long thin part, that sequence matters more than the grade.

Stainless 303 and 304 cut predictably with the right feed. Too light a feed and the surface work-hardens, which dulls the next pass. Grade 17-4PH in the H900 condition is harder and slower, but holds tolerance well. For medical parts, 316L is common and machines cleanly as long as coolant reaches the cut.

Titanium and Inconel sit at the difficult end. Heat stays at the tool edge, so speeds drop and tool life shortens. Ti-6Al-4V needs sharp tools, high-pressure coolant, and conservative depth of cut. Inconel is worse. Expect longer cycle times and plan for them in the quote rather than discovering them on the floor.

Plastics behave differently again. POM and PEEK cut cleanly but move with temperature, so measure after the part cools. Carbon fibre needs diamond or coated tooling to avoid delamination at the edge. ABS and PC are soft enough that clamping marks, not tolerance, usually set the limit.

• 1
  AluminiumFast and stable, watch stress movement in 7075
• 2
  StainlessAvoid light feeds, they work-harden the surface
• 3
  TitaniumHeat at the edge, slower speeds, shorter tool life
• 4
  PlasticsMeasure after cooling, clamping marks set the limit