How to Calculate CNC Machining Time

• 1
  Five things to know before you estimate
• 2
  What CNC machining time includes
• 3
  The basic formula for calculate CNC machining time
• 4
  Setup, fixturing, and non-cut time
• 5
  How material changes the estimate
• 6
  Six steps to build the estimate
• 7
  Typical parameters and what they do to the estimate

CNC machining time is the clock time a part occupies a machine, from raw stock to a finished, inspected component. For a milling job it covers the cut itself, the rapid moves between features, tool changes, and any probing. For a turned part it also covers bar feed and part transfer.

Engineers often quote only the cutting minutes and then wonder why the shop's number is higher. The gap is the non-cut portion, and on small parts it is usually the larger share.

A useful estimate splits the total into four buckets: cut, non-cut motion, tool change, and setup. Each bucket has its own drivers, so each can be argued about separately when a quote looks high.

Add inspection and any post-processing on top if the part needs anodizing, plating, or heat treatment. Those are calendar days, not spindle minutes, and they should be tracked apart from the machining estimate.

• 1
  Cut timeToolpath length divided by feed rate, summed over every operation.
• 2
  Non-cut motionRapids, retracts, and safe-Z moves between features.
• 3
  Tool change and setupPer cycle and per batch respectively; setup does not shrink with volume.
• 4
  Inspection and finishingCMM checks, deburring, anodizing, plating, and their queue time.

The starting point is simple: cutting minutes equal total cutting distance in millimeters divided by feed rate in millimeters per minute. If a 2,400 mm contour runs at 600 mm/min, that feature takes 4 minutes.

Feed rate comes from the tooth load and the spindle speed. For a 4-flute carbide end mill at 0.05 mm per tooth and 8,000 rpm, feed is 0.05 × 4 × 8,000 = 1,600 mm/min. Cut that in half for finishing passes and the same path costs twice as much.

For turning, use feed per revolution instead. At 0.2 mm/rev and 1,200 rpm, the tool advances 240 mm/min. A 300 mm long pass then takes 1.25 minutes.

Rapids are not free either. A machine running at 30,000 mm/min covers 500 mm of rapid in one second, but acceleration and deceleration at each corner means the real average is often closer to 15,000–20,000 mm/min.

• 1
  MillingCut minutes = path length (mm) ÷ feed (mm/min).
• 2
  TurningFeed (mm/min) = feed per rev (mm/rev) × rpm.
• 3
  DrillingCut minutes = depth ÷ (feed per rev × rpm).
• 4
  Pocket clearingUse stepover width to get the real number of passes, not one path.

Setup is charged per operation, not per part. A vise-mounted 3-axis job with three faces to machine needs three setups. A 5-axis part held once in a self-centering vise needs one. That difference can be 30 to 60 minutes on the first article.

Fixturing is where new designs lose days. Soft jaws, a custom plate, or a vacuum fixture can take 2 to 8 hours to design, cut, and prove out. Repeat orders reuse the fixture, so the per-part setup drops sharply from the second run onward.

In-cycle probing adds 10 to 40 seconds per feature but removes a manual check later. On tight-tolerance work at ±0.005 mm, that trade usually pays for itself.

Batching matters too. Running 50 parts from one setup spreads the setup minutes across 50 pieces. Running 5 parts does not, so small quantities always carry a higher per-part overhead.

• 1
  Count setups firstEvery new face or datum needs its own setup and its own error stack.
• 2
  Fixture design is real workBudget 2–8 hours for a custom fixture on a new geometry.
• 3
  First article costs moreSetup and prove-out dominate the first part, not the cut.
• 4
  Batch to dilute setupThe same setup spread over more parts lowers unit cost.

Aluminium 6061 cuts fast. Surface speeds of 300 to 500 m/min are normal with carbide, and a 12 mm end mill can run at 1,500 to 3,000 mm/min in roughing without chatter.

Stainless 304 and 316 work-harden, so feeds stay lower and coolant is mandatory. Expect surface speeds around 100 to 150 m/min and roughly 40 to 60% of the aluminium feed rate for the same tool.

Titanium Ti-6Al-4V is worse. Surface speed drops to 40 to 70 m/min, and tool life becomes the limiting factor rather than spindle speed. Many shops change inserts mid-cycle on long titanium parts, which adds minutes that never appear in the formula.

Tool steel and Inconel push surface speeds to 25 to 50 m/min with coated carbide. On these materials, the cut time estimate is only as good as the tool-life assumption behind it.

• 1
  AluminiumRough at 1,500–3,000 mm/min with a 12 mm carbide tool.
• 2
  Stainless 304/316Run 40–60% of the aluminium feed; keep the tool moving.
• 3
  Titanium Ti-6Al-4V40–70 m/min surface speed; watch insert wear.
• 4
  Inconel and tool steel25–50 m/min; expect tool changes inside the cycle.