📐 Free Gage Block Calculator — no login. Open it →

← AskMachinist · Guides · Calculator · 🔎 Search

Machining Cycle Time Estimate

Guide · Updated October 28, 2026

Cut time is the length the tool travels while cutting divided by the feed rate. For a quote you also add the approach and overtravel distance, rapid moves, tool changes and part handling. A quick estimate from speeds and feeds is usually close enough to quote a job and to see which operation dominates the cycle.

Need an exact reference size?

Build any gage block stack with the free Gage Block Calculator. Free, no login.

Step by step

  1. Find rpm: rpm = 3.82 × SFM ÷ diameter (inches).
  2. Find feed rate: Turning and drilling: ipm = rpm × feed per rev. Milling: ipm = rpm × teeth × chip load.
  3. Find length of travel: Length of cut plus approach and overtravel; for drills add the point length.
  4. Divide: Time (min) = length ÷ ipm, times the number of passes.
  5. Add non-cut time: Rapids, tool changes, probing and load/unload.
  6. Check on the first part: Compare with the control run timer and update the estimate.

The formulas

3.82 is 12 ÷ π rounded. For a face mill or end mill going all the way through a cut, the approach is about the cutter diameter (half to enter, half to clear) when the cutter is centered on the work.

Worked example: turning

Turn a 2.000 in diameter, 6 in long steel shaft at 500 SFM with 0.008 in/rev. rpm = 3.82 × 500 ÷ 2 = 955. Feed rate = 0.008 × 955 = 7.64 ipm. One pass = 6 ÷ 7.64 = 0.79 min. Three roughing passes and one finish pass at 0.004 in/rev (3.82 ipm, 1.57 min) total about 3.9 min of cutting. The finish pass is a large share, which is why a wiper insert that allows double the feed can pay off.

On a CNC with constant surface speed, rpm rises as the diameter gets smaller, so later passes are a little faster than this estimate.

Worked example: face milling

A 3 in face mill with 5 inserts runs at 600 SFM and 0.004 in per tooth across a 10 in long block. rpm = 3.82 × 600 ÷ 3 = 764. Feed = 764 × 5 × 0.004 = 15.3 ipm. Travel = 10 + 3 = 13 in, time = 0.85 min per pass.

Worked example: drilling

Drill eight 1/2 in holes 1.00 in deep in steel at 80 SFM and 0.006 in/rev. rpm = 611, feed = 3.67 ipm. Each hole travels 1.00 + 0.15 point + 0.05 clearance = 1.20 in, or 0.33 min, so eight holes are 2.6 min plus rapids between holes. With a peck cycle add the retract time, which can double cut time on deep holes.

Quoting tip

Add up cut time per operation, then add setup time spread over the lot. A part with 6 min of cutting and 2 min of handling, on a 2 hour setup for 40 parts, takes about 8 + 3 = 11 min per part.

Common problems

Leaving out approach and overtravel, using the starting diameter rpm for a whole CSS turning cycle, forgetting finish passes and spring passes, and ignoring rapid and tool change time on small parts where they dominate.

FAQ

How do I calculate cut time?

Time = length of travel ÷ feed rate in in/min.

How do I get feed rate in milling?

rpm × number of teeth × chip load per tooth.

Why is my CNC faster or slower than the estimate?

Acceleration, CSS rpm changes, rapids and feed override all change real cycle time.

How do I check first-part size?

Check the gage itself before trusting a measurement: gage blocks set mics, calipers and indicators; build any stack free at gageblockcalc.com.

Related guides and calculators

Build your stack in seconds

The free Gage Block Calculator finds the fewest-block combination for inch and metric sets, with wear blocks. No login.

Questions? Ask a machinist.

General shop information only — follow your drawing, tool maker's data and your quality system.