Machining time calculation (turning, milling, drilling)
Calculate the machining time t_h for longitudinal turning, peripheral/face milling and drilling into solid material: from tool geometry, cutting speed vc or spindle speed n, and feed f or feed per tooth fz you get the spindle speed, feed rate, total feed travel and the pure cutting time per workpiece - including plausibility warnings and a min:s display.
Calculation
Sketch: composition of the total feed travel L
Your inputs stay in your browser - all calculations run locally, nothing is sent to a server.
Formulas and fundamentals
Machining time and non-productive time
The machining time t_h is the pure cutting time during which the tool is actually engaged and removing material. Tool changes, setup, clamping, positioning and measuring, on the other hand, count as non-productive time - it depends on the machine, fixture and organization and is not part of this calculation. Machining time plus non-productive time together give the total production time per workpiece.
Spindle speed and cutting speed
Spindle speed and cutting speed are related via the tool or workpiece diameter d; depending on which is given, the calculator converts in the other direction:
Machining time for longitudinal turning
In longitudinal turning, the tool travels beyond the turning length l with an additional approach l_a (until fully engaged) and an overtravel l_u (free run-out, set to 0 e.g. at a shoulder). The total feed travel per cut is therefore L = l + l_a + l_u; for i cuts (e.g. roughing in several passes) the machining time follows as:
Machining time for milling
In peripheral or face milling, the feed per tooth fz, the tooth count z and the spindle speed n give the feed rate vf = fz·z·n. With the same total feed travel L = l + l_a + l_u (in milling the approach is often on the order of half the cutter diameter d/2, so the cutter is already fully engaged before reaching the workpiece edge), the machining time follows as:
Machining time for drilling into solid material
When drilling into solid material, the drill point is only fully engaged after the approach allowance l_s. For the standard point angle σ = 118°, l_s follows from the cone geometry of the point (half the diameter divided by the tangent of half the point angle):
With the total feed travel L = l + l_s + l_u (overtravel l_u only for through holes, otherwise 0) and k identical holes, the machining time follows as:
Multiple cuts when roughing and the link to the cutting-data calculator
If the allowable depth of cut ap is not enough to remove the full stock allowance in one pass, roughing is done in i = allowance/ap cuts (passes) - each additional cut extends the machining time proportionally. Suitable values for vc, f or fz and ap by material and cutting tool material are provided by the cutting-data calculator; this calculator takes over the kinematics and derives the resulting time from them.
Worked example
Worked example, turning: workpiece diameter d = 50 mm, turning length l = 100 mm, approach l_a = 2 mm, overtravel l_u = 2 mm, cutting speed vc = 200 m/min, feed f = 0.2 mm/rev, one cut (i = 1). The speed is n = 1000·200/(pi·50) = 1273.24 rpm, the total feed travel L = 100 + 2 + 2 = 104 mm. The machining time is t_h = 104·1/(0.2·1273.24) = 0.408 min ≈ 24.5 s.
Roughing in two passes with the same feed (i = 2, e.g. because the stock allowance exceeds the allowable depth of cut ap) would double the machining time to t_h ≈ 0.816 min ≈ 49 s - the total feed travel L stays the same, only the number of cuts i enters t_h linearly.
The same kinematics apply to milling and drilling, with a different feed quantity: for a cutter with d = 63 mm, z = 5 teeth, milling length l = 150 mm, approach l_a = 32 mm (suggested d/2), overtravel l_u = 2 mm, vc = 180 m/min and fz = 0.1 mm, this gives n = 909.46 rpm, v_f = 454.73 mm/min and t_h = 184/454.73 = 0.4046 min. For a hole with d = 8.5 mm, l = 25 mm, vc = 30 m/min, f = 0.15 mm/rev and k = 4 identical holes (approach allowance l_s = 0.3·8.5 = 2.55 mm), n = 1123.45 rpm and t_h = 4·27.55/(0.15·1123.45) = 0.654 min.
Frequently asked questions
What is the difference between machining time and non-productive time?
The machining time t_h is exclusively the cutting time during which the tool actually removes material - that is exactly what this calculator computes. Tool changes, setup, clamping and unclamping, rapid positioning moves and measuring count as non-productive time; it depends on the machine, fixture, programming and organization and cannot be calculated in general. Total production time per workpiece is always machining time plus non-productive time.
Where do the values for cutting speed vc and feed f come from?
Cutting speed and feed depend on the material, cutting tool material, tool geometry and desired tool life - reference tables from tool manufacturers provide guideline values for these. This calculator takes vc or n and f/fz as given values and only calculates the resulting kinematics and time from them; choosing the cutting values themselves is the job of the cutting-data calculator (turning/milling/drilling) with material guideline values.
Why is an approach allowance needed when drilling?
A twist drill has a conical point (standard point angle 118°). Before the full drill diameter is engaged, the point must first fully plunge in - this additional travel l_s = 0.3·d (from the cone geometry: (d/2)/tan(59°)) is added to the actual drilling depth, otherwise the machining time would be systematically underestimated.
How many cuts are needed when roughing?
The number of cuts (passes) i follows from the stock allowance to be removed divided by the allowable depth of cut per pass ap: i = allowance/ap, rounded up to a whole number. Each additional cut extends the machining time proportionally (t_h scales linearly with i), since the same feed travel is traversed multiple times.
Does the calculation apply equally to CNC and conventional machines?
Yes, the kinematics (speed, feed rate, travel, time) are machine-independent and apply equally to conventional and CNC-controlled machines. Differences between machine types mainly show up in the non-productive time (tool changes, program execution, setup), which is deliberately not included here.
How do I use this to calculate the cycle time of a manufacturing operation?
The cycle time of an operation follows from the sum of all machining times (possibly for several tools/cuts) plus the non-productive times per workpiece (tool changes, clamping, measuring, non-cutting program runtime). This calculator provides the machining-time building blocks for that; the non-productive times must be added based on the specific shop and machine, for example using the axis move & cycle time calculator for pure positioning axes.
Related tools
Cutting data calculator
Pro exportDetermine cutting speed, spindle speed and feed for turning, milling and drilling.
Cutting Force & Power (Kienzle)
Pro exportDetermine cutting force, power and machining time for turning, milling and drilling with the Kienzle model.
Tapping Drill & Clearance Hole
Pro exportDetermine tapping drill diameters for metric threads per DIN 13 and clearance holes per EN 20273.