CNC processing technology: how metal removal actually works

• 1
  Key takeaways
• 2
  What CNC processing technology removes, and how
• 3
  Where your ±0.005 mm actually goes
• 4
  Why setup count decides your part cost
• 5
  How the fixture changes what the machine can hold
• 6
  How material choice narrows the process window
• 7
  How measurement defines what you actually get
• 8
  CNC processing technology: machine choice by part geometry

Every CNC operation is a controlled fracture. A cutting edge enters the workpiece, shears a chip off the surface, and leaves behind a new surface with a measurable roughness. The machine's job is to hold the tool and the part in a known relationship while that happens thousands of times per minute. Everything else, the controller, the coolant, the fixture, exists to keep that relationship stable.

The chip carries most of the heat away. If a chip is thin and long, heat leaves with it and the part stays cool. If the chip is thick or the tool rubs instead of cutting, heat goes into the workpiece, and the workpiece grows. A 100 mm aluminum block can move 0.02 mm from a 10 °C rise. That is four times the ±0.005 mm tolerance we hold on finish passes.

Cutting speed, feed per tooth and radial engagement set the chip load. On 6061-T6 aluminum, a 12 mm carbide end mill typically runs 3,000–8,000 rpm with 0.05–0.15 mm feed per tooth. On 316 stainless, the same tool drops to 800–1,500 rpm with 0.03–0.08 mm per tooth. Push beyond that and the edge chips. Back off too far and the tool rubs, work-hardens the surface, and the next pass cuts through a harder skin.

Roughing and finishing are separate decisions. Roughing removes bulk with the largest tool that fits, leaving 0.3–0.5 mm of stock. Finishing removes that stock in one continuous pass with a sharp tool at high spindle speed and low feed. Mixing the two, such as taking a light finishing cut with a worn roughing tool, is the most common cause of poor surface finish we see in first-article inspection.

• 1
  Chip loadFeed per tooth × teeth × rpm = table feed. Set it before spindle speed.
• 2
  Radial engagementBelow 10% of tool diameter keeps heat in the chip on deep cuts.
• 3
  CoolantThrough-spindle coolant matters most in deep pockets and titanium.
• 4
  Tool runoutAbove 0.01 mm runout, one flute does most of the cutting.

A ±0.005 mm callout is a budget, and the machine spends it in several places. Machine geometry contributes a few microns. Tool deflection under cutting load adds more. The fixture adds its own error if the part moves during clamping. Thermal growth of the part, the tool and the spindle adds the rest. On a small part in a temperature-controlled shop, those add up to roughly 0.003–0.006 mm, which is why we hold ±0.005 mm and inspect 100% before shipment.

The budget changes with part size. On a 4,000 mm part, thermal drift alone can exceed the tolerance band, so we either cut in a temperature-stable window or measure and compensate. On a 50 mm part, the dominant error is usually tool deflection, not the machine. That is why a smaller tool with a shorter flute length often holds tighter tolerance than a larger, stiffer tool.

Surface finish and tolerance trade against each other. Ra 0.2–0.8 μm usually requires a dedicated finishing pass with a sharp tool and a light feed. Ra 1.6–3.2 μm is achievable in a single pass on many materials. If a drawing asks for both a tight bore and a fine finish on the same feature, expect two operations and a longer cycle.

Material behavior sets the floor. Aluminum 6061 and 7075 hold tight tolerance well because they cut cleanly and conduct heat fast. Titanium Ti-6Al-4V work-hardens and moves more, so we plan extra finishing passes and slower feeds. Inconel is worse again. Tight tolerance on Inconel is possible, but the process window narrows and the cycle time grows.

• 1
  Small partsTool deflection dominates. Use shorter, smaller tools.
• 2
  Large partsThermal drift dominates. Control the shop temperature.
• 3
  Thin wallsClamping force and springback dominate. Plan support ribs.
• 4
  Deep boresTool shank stiffness dominates. Step down with a boring head.

Each time a part leaves the machine and comes back, the operator has to locate it again. A setup that repeats to 0.02 mm is normal. A setup that repeats to 0.005 mm requires a dedicated fixture and a probe. That is the real reason 5-axis machining costs more per hour but often costs less per part: it removes setups.

Consider a bracket with features on four faces. On a 3-axis machine, that is four setups, four re-clamps, and four chances to lose position. On a 5-axis machine with a Ø400 mm rotary table, it is one setup. The cycle time may be longer because the tool has to reach around the part, but the total time from raw stock to finished part often drops because setup and re-fixturing time disappears.

The trade-off flips on simple parts. A flat plate with holes from one direction does not benefit from 5-axis. The extra axes add programming time, and the machine's higher hourly rate buys nothing. For parts like that, 3-axis milling and a good vise will be faster and cheaper.

Mill-turn centers sit between the two. They combine turning and milling in one setup, which suits shafts, housings and parts with a rotational axis and side features. If your part has a turned diameter plus milled flats or cross-holes, a mill-turn center usually beats two separate operations.

• 1
  3-axisBest for prismatic parts with features from one or two directions.
• 2
  4-axisBest for parts with a rotational axis and side features.
• 3
  5-axisBest when four or more faces need tight positional relationships.
• 4
  Mill-turnBest for turned bodies with milled features in one cycle.

The fixture is part of the machine's error budget. A vise with 0.02 mm jaw parallelism cannot produce a 0.005 mm parallel face, no matter how good the spindle is. Soft jaws bored in place fix that. So do dedicated fixtures machined on the machine that will run the part.

Thin parts are the hard case. A 2 mm aluminum wall deflects under clamping force. Once the vise releases, the part springs back and the wall is no longer straight. We handle this by supporting the wall with a sacrificial block, using low-pressure clamps, or cutting the wall in a finishing pass after all other stock is removed.

For parts that cannot be clamped from outside, vacuum chucks and adhesive fixturing work. They hold flat, thin parts without distorting them. The limit is cutting force: vacuum holding is fine for light finishing passes, not for heavy roughing.

Probing closes the loop. A spindle probe measures the raw stock before cutting and the finished feature after cutting. If the stock is 0.3 mm oversize, the controller shifts the tool path. If the finished bore is 0.004 mm small, the operator knows before the part leaves the machine. This is how we keep first-article pass rates high on tight-tolerance runs.

• 1
  Soft jawsBore them in place on the machine that runs the job.
• 2
  Vacuum chucksGood for thin plates, light cuts only.
• 3
  Adhesive fixturingGood for fragile parts, slow to set up.
• 4
  In-process probingCatches drift before the part is finished.

Aluminum is the default for prototypes and many production parts. 6061-T6 machines cleanly, welds well and anodizes predictably. 7075 is stronger but more prone to distortion after machining because of residual stress in the plate. If you need 7075 flatness, plan a stress-relief step or accept a longer finishing sequence.

Stainless 303 and 304 cut differently. 303 has sulfur added for chip breaking and machines fast. 304 galls, work-hardens and needs lower surface speed and more coolant. 316 and 316L resist corrosion better but are harder again. 17-4PH in the H900 condition is strong and machinable but requires care on finishing passes to avoid a work-hardened skin.

Titanium and Inconel sit at the difficult end. Ti-6Al-4V has low thermal conductivity, so heat stays in the tool. Cutting speeds drop to 30–60 m/min for carbide. Inconel 718 is worse, with speeds of 20–40 m/min. Both materials need rigid setups, sharp tools and generous coolant. The payoff is strength-to-weight and heat resistance that aluminum and steel cannot match.

Plastics behave differently again. POM and PEEK machine well but move with temperature. PMMA and PC can craze if coolant chemistry is wrong. Carbon fiber reinforced plastic is abrasive and wears tools quickly, so we plan for more tool changes and a dust extraction setup.

• 1
  AluminumFast, predictable, good for tight tolerance.
• 2
  StainlessWatch work hardening, especially 304 and 316.
• 3
  TitaniumSlow speeds, rigid setup, plenty of coolant.
• 4
  PlasticsControl temperature and coolant chemistry.

A tolerance is only meaningful if you can measure it. A caliper reads to 0.02 mm. A micrometer reads to 0.001 mm but only on outside diameters. A coordinate measuring machine (CMM) reads position, form and orientation across a full part. If your drawing calls for ±0.005 mm position, the inspection method has to be capable of reading better than that.

We inspect raw material before cutting, monitor in process, and inspect 100% of parts before shipment. Reports are available on request. For critical features, we use a CMM and record the actual values, not just pass/fail. That data is what lets us hold 99.99% qualification rate across production runs.

The measurement loop also catches drift. If the first ten parts of a run measure 0.002 mm above nominal, we adjust the tool offset before the eleventh. Without that loop, a small thermal drift becomes a rejected batch by the end of the shift.

For prototypes, inspection often matters more than the part itself. A first article that measures well tells you the design is manufacturable. A first article that measures poorly tells you where to add tolerance or change a feature before you commit to tooling.

• 1
  Caliper±0.02 mm. Good for reference, not for tolerance.
• 2
  Micrometer±0.001 mm. Outside diameters and thickness only.
• 3
  CMMPosition, form and orientation. Use for tight callouts.
• 4
  In-process probeCatches drift before the part is finished.