Skip to content
Engineering Bible

Results appear as you type. Use the arrow keys to move through them and Enter to open one.

Popular

↑ ↓ moveEnter openEsc close

Machining time calculator (turning, facing, drilling, milling)

Cutting time per pass and per part for turning, facing, drilling and milling from length, feed and rpm, and total job time with set-up and handling.

Units

Results are estimates. They do not replace the governing code, class or flag requirements, or a check by a competent person. Report a problem

Introduction

Cutting time is the distance the tool feeds divided by the feed rate. On a lathe or a drill, the feed rate is the feed per revolution times the rpm. Turning 100 mm plus 3 mm of approach at 0.2 mm/rev and 1 000 rpm takes 103 ÷ 200 = 0.515 min. A milling cutter feeds at chip load × teeth × rpm.

This calculator gives the tool travel, the feed rate and the cutting time of one pass, the time per part for several passes, and the total job time for a batch with set-up and handling time. It covers turning, facing, drilling and milling. It is for machinists, CNC programmers and estimators quoting jobs and planning shifts.

Formulas

Feed rate:

turning, facing, drilling:  v_f = f × n
milling:                    v_f = f_z × z × n

Tool travel per pass:

turning, milling:  L_t = L + approach and overtravel
facing:            L_t = (D − d) / 2 + approach
drilling:          L_t = depth + D / (2 tan(θ/2)) + approach

Times:

t_pass = L_t / v_f
t_part = passes × t_pass
t_job = set-up + parts × (t_part + handling)
  • f — feed per revolution; f_z — feed per tooth; z — number of teeth; n — spindle speed
  • L — length of cut; D — outside or drill diameter; d — bore diameter; θ — drill point angle

Assumptions and limitations

  • The tool feeds at a constant rate over the whole travel. Rapid moves, tool changes and acceleration belong in the handling time per part.
  • Facing runs at a constant rpm. A lathe with constant surface speed raises the rpm towards the centre and finishes the face sooner.
  • Drilling adds the length of the drill point, so the full diameter reaches the stated depth. For a through hole, the approach and overtravel should include the breakthrough.
  • In milling, the travel is the path of the cutter centre. A face mill must travel its own diameter past the part to clear the surface completely.
  • Spindle speeds and feeds come from the speeds and feeds calculator or the tool maker's data.

Worked example

A shaft is turned over 100 mm with 3 mm of approach and overtravel. The feed is 0.2 mm/rev at 1 000 rpm, in two passes. A batch of 50 parts needs 30 min of set-up and 0.5 min of handling per part.

  1. Feed rate: 0.2 × 1 000 = 200 mm/min.
  2. Time per pass: 103 / 200 = 0.515 min.
  3. Time per part: 2 × 0.515 = 1.03 min of cutting, 1.53 min with handling.
  4. Job time: 30 + 50 × 1.53 = 106.5 min, about 1.8 hours.

After set-up, the lathe makes about 39 parts an hour.

FAQ

How do I calculate machining time?

Divide the tool travel by the feed rate. The feed rate is feed per revolution times rpm, or chip load times teeth times rpm for milling.

What is approach and overtravel?

The extra distance the tool feeds before it enters and after it leaves the cut. A milling cutter that must clear the work needs more than a lathe tool.

How do I estimate drilling time?

Add the drill point length to the depth: about 0.3 × the diameter for a 118° drill. Then divide by feed per revolution times rpm.

Why is my real cycle time longer than the calculated cutting time?

Rapids, tool changes, spindle starts, measuring and loading all add time. Put them in the handling time per part.

What is floor-to-floor time?

The time from picking up a raw part to putting down a finished one. It is cutting time plus handling.

How do I reduce machining time?

Raise the feed or the cutting speed within the tool's limits, take fewer, deeper passes, and shorten the approach. Set-up time matters most for small batches.

Related calculators

What this calculator is checked against

Before every release the calculator must reproduce each case below. The note under each case says where the expected answer comes from: a standard, a textbook, a published table, or a hand calculation shown in full.

  1. Turning 100 + 3 mm at 0.2 mm/rev and 1 000 rpm: 103 / 200 = 0.515 min a pass; 2 passes 1.03 min; 50 parts + 30 min set-up + 0.5 min each = 106.5 minGroover / Kalpakjian: T_m = L / (f N) (hand calculation)
  2. Drilling 1 in deep with a 1/2 in 118° drill: point 0.1502 in + 0.1 in approach = 1.2502 in at 0.008 in/rev and 800 rpm takes 0.1954 minPoint length D / (2 tan 59°) = 0.3004 D; T = L / (f N) (hand calculation)
  3. Facing a 2 in bar to the centre with 0.1 in approach at 0.008 in/rev and 800 rpm: 1.1 in at 6.4 in/min = 0.1719 min; a 1 in bore leaves 0.6 inTravel (D − d)/2 + allowance (hand calculation)
  4. Milling 4 + 0.1 in at 0.003 in/tooth, 4 teeth, 800 rpm: 9.6 in/min, 0.4271 min; three passes take three times as longGroover: f_r = N n_t f, T_m = (L + A) / f_r (hand calculation)
  5. A bore as large as the outside, zero travel, fractional passes and zero rpm are rejected; facing warns about constant rpmBehaviour check: warnings and rejected inputs
  6. Worked example of the article: the calculator reproduces 0.515 min, 1.03 min, 106.5 min to the digits printedThe worked example on this page, to the digits printed

Assumptions and sources

Assumptions and limits

  • The tool feeds at a constant rate over the whole travel: the length of cut plus the approach and overtravel you enter; rapid moves, tool changes and acceleration are part of the handling time.
  • Facing runs at a constant spindle speed from the outside diameter to the centre (or to the bore); a lathe with constant surface speed raises the rpm towards the centre and finishes sooner.
  • Drilling travel adds the length of the drill point, D / (2 tan(θ/2)), so that the full diameter reaches the stated depth; add the breakthrough allowance for a through hole.
  • In milling the travel is the path length of the cutter centre; for a face mill to clear the part completely the overtravel must include the cutter diameter.

Sources

  • Groover, M. P., Fundamentals of Modern Manufacturing, Wiley, chapter on machining operations: T_m = L / f_r with f_r = N f (turning, drilling) and T_m = (L + A) / f_r with f_r = N n_t f (milling)
  • Kalpakjian, S. and Schmid, S. R., Manufacturing Engineering and Technology, 7th ed., Pearson: cutting time t = l / (f N) for turning and drilling

Cite this calculator

Papandreou, C. (2026). Machining time calculator (turning, facing, drilling, milling). Engineering Bible. https://engineeringbible.com/manufacturing/machining-time/

Embed this calculator on your site

Copy this HTML into your page. The calculator stays free to use and links back here.

By Christos Papandreou. Updated . How the numbers are checked.