How to use this calculator
- Choose the feed model. Use direct feed rate, milling feed from RPM/flutes/chip load, or turning feed from RPM/feed per revolution.
- Enter the feed travel. Enter cutting length, approach and overtravel. These are the distances run at feed.
- Enter passes and batch size. Use the number of repeated passes per part and the run quantity.
- Add non-cut time. Add rapids, tool changes, dwell, probing or handling time per part.
- Use the result. Read feed time, cycle time each, batch time and parts per hour.
How it works
Machining time starts with the distance that actually runs at feed:
Lfeed = Lcut + Lapproach + Lovertravel
If you already know the programmed feed rate, use it directly. For milling, the table feed comes from spindle speed, flutes and chip load:
Vf = n · Z · fz
For turning-style or drill-style feed per revolution, the feed rate is:
Vf = n · fn
Feed time is then distance divided by feed rate. The calculator multiplies that by the number of passes, then adds the non-cut allowance:
cycle_each = passes · Lfeed / Vf + non_cut_time
Worked example
Verified against the live calculator
Mill a 200 mm slot with 12 mm approach,
12 mm overtravel, 2 passes, a 4-flute cutter
at 6000 rpm and 0.08 mm/tooth chip load. Add
30 s non-cut time per part and quote 25 parts.
Feed rate is 6000 × 4 × 0.08 = 1920 mm/min. Feed distance per pass is
200 + 12 + 12 = 224 mm. Time per pass is
224 / 1920 = 0.1167 min = 7.0 s, so two passes take
14.0 s. With 30 s non-cut time, cycle time is
44.0 s per part, or 18.3 min for 25 parts.
Frequently asked questions
How do you calculate CNC machining time?
For a constant-feed move, machining time is feed distance divided by feed rate. The feed distance is the cutting length plus any approach and overtravel. Multiply by the number of passes, then add rapids, tool changes, dwell or handling time as a separate non-cut allowance.
How do you calculate milling feed rate from RPM and chip load?
Milling feed rate is Vf = n × Z × fz, where n is spindle RPM, Z is the number of effective flutes, and fz is chip load per tooth. That feed rate is then used in time = distance ÷ feed.
How do you calculate turning time?
Turning-style feed time uses feed per revolution: Vf = n × fn. The cutting time is machined length divided by that feed rate, multiplied by the number of passes.
Does this replace CAM simulation?
No. It is a planning estimator for straight feed moves and quote checks. CAM backplots and machine control reports capture acceleration, rapids, retracts, tool changes, cutter comp, probing and canned-cycle behavior more accurately.
How does this connect to machining cost?
Use the cycle time each from this page as the cycle-time input in the machining cost calculator. Keep setup time, material, tooling and secondary work separate so the cost breakdown stays visible.
Method & assumptions
- This is constant-feed planning math. It does not model acceleration, deceleration, machine dynamics, controller look-ahead or smoothing.
- Approach and overtravel are counted only if they run at feed. Rapid moves belong in the non-cut time allowance.
- For milling, use the CNC speeds and feeds calculator or chip load calculator to sanity-check feed rate before estimating time.
- For holes, the drilling feed rate calculator includes drill-point allowance and hole count.
- Use the cycle time each in the machining cost calculator when turning runtime into part cost.