How to Use a CNC Machin to Cut Parts That Hold Tolerance

• 1
  Key takeaways
• 2
  What Has to Be Decided Before the First Cut
• 3
  Feeds, Speeds, and What the Chip Tells You
• 4
  Which Materials Cut Cleanly and Which Fight Back
• 5
  Holding ±0.005 mm and Knowing When It Is Not Realistic
• 6
  Step by Step: How to Use a CNC Machin to Cut a Part
• 7
  When to Cut It and When to Choose Another Process

A cnc machin to cut metal is only as good as the decisions made before the spindle turns. The CAD model arrives as STEP or IGES, and the first job is to check whether it can actually be held, reached, and measured. We look at the smallest internal corner, the deepest pocket, and the datums the drawing calls out. If a 3 mm end mill has to reach 40 mm deep, the tool will deflect and the cut will drift.

Stock selection comes next. Oversize stock gives room to clean up a sawn face, but it also means more roughing time and more material to stress-relieve. For 6061-T6 plate, we usually leave 0.5–1.0 mm per side on critical faces. For 17-4PH or 4140 in a hardened state, the allowance is smaller and the cutting strategy changes to light radial passes.

Workholding is where most first articles fail. A vise with 2 mm of grip on a tall part will lift it. Thin plate needs a vacuum fixture or tabs. A part with a 4,000 mm length needs multiple setups or a large-travel machine. If the fixture cannot resist the cutting force, no amount of CAM tuning saves the job.

• 1
  Check tool reach firstDepth-to-diameter above 4:1 on a small end mill means step down or change the design.
• 2
  Pick datums you can touchA datum on a curved surface cannot be probed or indicated reliably.
• 3
  Decide the finish before roughingRa 0.8–1.6 μm needs a separate finishing pass at low stepover.

The controlling number on a cnc machin to cut steel or aluminium is chip load per tooth, not spindle RPM. A 10 mm three-flute carbide end mill in 6061 might run 8,000 rpm at 0.10 mm per tooth, which gives a feed of 2,400 mm/min. In 4140 at 28 HRC, the same tool drops to about 2,500 rpm and 0.05 mm per tooth. The chip should look like a comma, not dust and not a long ribbon.

Surface speed changes with material. Aluminium runs 300–500 m/min with carbide. Mild steel runs 120–180 m/min. Stainless 316 work-hardens, so we keep the radial engagement high enough to stay under the hardened layer, typically 30–40 percent of tool diameter. Titanium Ti-6Al-4V runs 40–60 m/min with flood coolant and a rigid setup.

When the cut sounds wrong, the cause is usually one of three things. A high-pitched squeal means chatter from low rigidity or too high a radial depth. A dull thud means the tool is rubbing instead of cutting. Fine dust instead of chips means the feed is too low for the RPM, which polishes the edge and kills tool life fast.

• 1
  Start conservative on the first partReduce feed by 20 percent, then raise it once the sound and chip shape are right.
• 2
  Coolant choice mattersFlood for titanium and stainless, air blast for aluminium, mist only as a last resort.

Aluminium 6061 and 6082 are the easiest metals to cut on a machining center. They machine at high speed, hold ±0.005 mm on well-supported features, and take an Ra 0.8 μm finish without special tooling. 7075 is stronger but more prone to leaving a gummy edge on a dull cutter, so tool changes come sooner. ADC12 die-cast stock can have porosity that shows up as a pinhole after anodizing.

Stainless 303 is free-machining and behaves well. 304 and 316 are a different story: they work-harden at the surface, so a light pass that rubs instead of cuts will make the next pass harder. 17-4PH in the H900 condition cuts cleanly but needs carbide and a rigid setup. 440C in a hardened state is usually ground after machining, not cut to final size.

Plastics bring their own problems. POM and ABS cut fast but melt if the chip cannot clear. PEEK needs sharp tooling and a slower feed to avoid stress marks. Carbon fibre is abrasive and wears carbide quickly, so we plan tool changes rather than waiting for a bad edge. Inconel and magnesium are both handled here, but each has its own rule set for speed and fixturing.

A ±0.005 mm tolerance is achievable on a rigid setup, with a sharp tool, and on a feature you can measure. It is not achievable on a 0.5 mm wall at the end of a long cantilever. When a drawing calls for a tight tolerance across a thin section, the cut itself is not the problem; the part moves after the tool passes.

Temperature matters at this level. A 100 mm aluminium part grows about 0.0023 mm per degree Celsius. If the shop is at 26 °C and the inspection room is at 20 °C, the measurement will drift. We inspect at a controlled temperature and note the reading conditions on the report.

Surface finish and tolerance are linked. Ra 0.2–0.8 μm usually needs a finishing pass with a small stepover and a fresh edge, which adds cycle time. Ra 1.6–3.2 μm is as-machined and comes off the rougher or a light finish pass. Tell us which surfaces actually matter, and we will not spend time polishing a mounting face that sits against a bracket.

• 1
  Tight tolerance on one feature onlyCall out the critical dimension instead of tightening the whole drawing.
• 2
  Add a datum you can probeA flat, accessible face shortens setup and inspection time.