Cutting data calculator for turning, milling and drilling
The calculator determines spindle speed n, feed rate vf, material removal rate Q and machining time t_h for the three basic operations. Reference values for the cutting speed vc are stored per material group and cutting tool; for turning the cutting force can additionally be estimated after Kienzle. All reference values are starting points for average conditions, and the tool manufacturer's data for the specific tool takes precedence, live with every input.
Calculation
Results
- Spindle speed n
- 1,459 1/min
- Cutting speed vc
- 275 m/min
- Feed rate vf
- 437.7 mm/min
- Removal rate Q
- 206.3 cm³/min
- Machining time t_h
- 0.283 min (17 s)
- Feed path L
- 124 mm
- nearest step
- 1,600 1/min
Cutting force and power (Kienzle)
- h
- 0.3 mm
- b
- 2.5 mm
- kc
- 2,184 N/mm²
- Fc
- 1,638 N
- Pc
- 7.51 kW
- P_M
- 9.39 kW
- M
- 49.1 Nm
Composition of the feed path L
Cutting speed reference table, vc in m/min
For looking up: stated are the starting value for normal machining conditions and, in smaller type next to it, the lower and upper limit. These book values do not enter the calculation; the calculator works with the curated ranges of the material selection above.
Turning
Longitudinal turning, roughing (depth of cut ap 2 … 4 mm), with carbide or HSS turning tool.
| Material group | Rm in N/mm² or hardness HB | vc carbide | vc HSS |
|---|---|---|---|
| Structural steel | Rm ≤ 500 | 220 (150…300) | 50 (40…60) |
| Structural steel | Rm > 500 | 170 (100…240) | 40 (30…50) |
| Free-cutting steel | Rm ≤ 570 | 200 (130…270) | 35 (30…40) |
| Case-hardening steel | Rm ≤ 570 | 210 (150…260) | 30 (25…35) |
| Quenched and tempered steel, unalloyed | Rm ≤ 650 | 190 (120…240) | 30 (25…35) |
| Quenched and tempered steel, alloyed | Rm ≤ 750 | 130 (90…180) | – |
| Tool steel | Rm ≤ 750 | 125 (85…170) | 20 (18…22) |
| Cast steel | Rm > 700 | 110 (80…140) | 17 (14…20) |
| Stainless steel, austenitic | Rm ≤ 680 | 110 (90…130) | 20 (18…22) |
| Cast iron with lamellar graphite | ≤ 200 HB | 280 (230…330) | 35 (30…40) |
| Cast iron with spheroidal graphite | ≤ 250 HB | 210 (160…260) | – |
| Aluminium wrought alloy | Rm ≤ 300 | 450 (380…520) | 140 (120…160) |
| CuZn alloy (brass) | Rm ≤ 600 | 270 (250…300) | 90 (80…100) |
| Thermoplastic, thermoset | – | 360 (270…450) | 225 (200…250) |
Milling
Carbide: 45° face milling with indexable inserts. HSS: cylindrical end mill, coated.
| Material group | Rm in N/mm² or hardness HB | vc carbide | vc HSS |
|---|---|---|---|
| Structural steel | Rm ≤ 500 | 275 (250…300) | 65 (60…70) |
| Structural steel | Rm > 500 | 235 (220…250) | 65 (60…70) |
| Free-cutting steel | Rm ≤ 570 | 250 (230…270) | 65 (60…70) |
| Case-hardening steel | Rm ≤ 570 | 230 (200…260) | 65 (60…70) |
| Quenched and tempered steel, unalloyed | Rm ≤ 650 | 230 (200…260) | 65 (60…70) |
| Quenched and tempered steel, alloyed | Rm ≤ 750 | 220 (190…250) | 55 (50…60) |
| Tool steel | Rm ≤ 750 | 135 (120…150) | 65 (60…70) |
| Cast steel | Rm > 700 | 160 (140…180) | 60 (55…65) |
| Stainless steel, austenitic | Rm ≤ 680 | 210 (190…230) | 27 (24…30) |
| Cast iron with lamellar graphite | ≤ 200 HB | 235 (220…250) | 55 (50…60) |
| Cast iron with spheroidal graphite | ≤ 250 HB | 215 (200…230) | 55 (50…60) |
| Aluminium wrought alloy | Rm ≤ 300 | 725 (600…850) | 350 (340…360) |
| CuZn alloy (brass) | Rm ≤ 600 | 550 (500…600) | 85 (80…90) |
| Thermoplastic, thermoset | – | 500 (400…600) | 325 (300…350) |
Drilling
Twist drills, carbide and HSS both coated.
| Material group | Rm in N/mm² or hardness HB | vc carbide | vc HSS |
|---|---|---|---|
| Structural steel | Rm ≤ 500 | 85 (70…100) | 50 (38…63) |
| Structural steel | Rm > 500 | 85 (70…100) | 37 (31…44) |
| Free-cutting steel | Rm ≤ 550 | 85 (70…100) | 37 (31…44) |
| Case-hardening steel, unalloyed | Rm ≤ 550 | 85 (70…100) | 37 (31…44) |
| Case-hardening steel, alloyed | Rm ≤ 750 | 75 (60…85) | 22 (19…25) |
| Quenched and tempered steel, unalloyed | Rm ≤ 650 | 85 (70…100) | 37 (31…44) |
| Quenched and tempered steel, alloyed | Rm ≤ 750 | 75 (60…85) | 21 (19…25) |
| Tool steel | Rm ≤ 750 | 75 (60…85) | 16 (13…19) |
| Stainless steel, austenitic | Rm ≤ 680 | 40 (30…50) | 19 (13…25) |
| Cast iron with lamellar graphite | ≤ 200 HB | 105 (80…130) | 31 (25…38) |
| Cast iron with spheroidal graphite | ≤ 250 HB | 85 (70…100) | 37 (31…44) |
| Aluminium wrought alloy | Rm ≤ 350 | 240 (180…300) | 87 (50…125) |
| CuZn alloy, short-chipping | Rm ≤ 600 | 170 (120…230) | 100 (75…125) |
| Thermoplastic | – | – | 30 (20…40) |
Source: Tabellenbuch Metall (Europa-Lehrmittel), chapter 6.6 on machining. Turning page 316 (carbide) and page 318 (HSS), milling page 324 (carbide) and page 326 (HSS), drilling page 332. Starting values for normal conditions; the tool manufacturer's data takes precedence.
Calculation in your browser, inputs go to our server only when you export or save.
Formulas and fundamentals
Kinematics: spindle speed and cutting speed
From the cutting speed vc and the governing diameter the spindle speed follows. For turning d is the workpiece diameter, for milling and drilling the tool diameter; the factor 1000 converts metres to millimetres. Conversely, a given spindle speed yields the cutting speed:
Feed
For turning and drilling the feed rate uses the feed per revolution f. For milling the teeth add up, using the feed per tooth fz and the number of teeth z; for z = 1 the milling formula reduces to the turning formula:
Material removal rate and machining time
The material removal rate is directly given in cm³/min. The drilling formula represents the geometrically removed volume; a simplification common in some reference books yields twice this value:
The machining time follows from the total feed path L per pass and the number of passes i:
The path L consists of approach, machining length and overtravel. For drilling the lead-in of the drill point is added, which for the standard point angle of 118° is about 0.3·d:
For longitudinal turning with an oblique lead angle κ < 90° the lead-in path is added as well, the distance the edge travels until full depth of cut; at κ = 90° it is zero:
For milling the cutter diameter is added or subtracted depending on the path convention.
Cutting force after Kienzle (turning)
From the chip thickness and the chip width the specific cutting force follows, and from it the cutting force with the chip cross section A:
The cutting power is Pc = Fc·vc/60000 in kW, the required machine power P_M = Pc/η, and the spindle torque M = Fc·d/2000 in Nm. The values kc1.1 and mc depend on the material and scatter noticeably between sources.
Calculating the cutting speed
The cutting speed vc is the relative speed between cutting edge and workpiece at the cutting diameter, given in m/min. It is not a machine setting but follows from the pairing of workpiece material and cutting tool material: you look up the reference value and derive the spindle speed n = vc·1000/(π·d).
The calculator accepts either input. In vc mode the cutting speed yields the target spindle speed; in n mode it works the other way round and returns the actual cutting speed vc = π·d·n/1000, the question that arises on a fixed machine speed step. The governing diameter is always the one being cut: the workpiece diameter for turning, the tool diameter for milling and drilling.
vc directly determines tool life, cutting temperature and surface finish. A reference range is therefore stored for every material group and cutting tool material and can be applied with one click; if the entered value lies outside that range, the calculator flags it as a note.
Calculating the feed
The feed is the distance the tool advances per revolution or per tooth in the feed direction. For turning and drilling this is the feed per revolution f in mm, for milling the feed per tooth fz in mm, multiplied by the number of teeth z.
Feed and spindle speed give the feed rate vf = f·n or vf = fz·z·n in mm/min. vf is the value the machine actually travels at; together with the feed path L and the number of passes i it yields the machining time t_h = L·i/vf.
The feed also sets the chip thickness h = f·sin κ and with it the cutting force and the roughness. A larger feed shortens the machining time almost proportionally but raises the cutting force and leaves a coarser surface. The calculator therefore states a reference range for f and fz per material group, and for drilling additionally as a multiple of the drill diameter.
Cutting speed reference table
Without manufacturer data at hand you first need a sound starting value. Below the calculator a reference table of the cutting speed is therefore given for each operation, covering the common pairings of material group and cutting tool material, separately for turning, milling and drilling.
Each entry states three numbers: the highlighted starting value for normal machining conditions plus the lower and upper limit. Unfavourable conditions such as long tool overhang, interrupted cut, poor cooling or a compliant setup lead to the lower value, favourable ones to the upper.
The values are taken from Tabellenbuch Metall (Europa-Lehrmittel), chapter 6.6 on machining. They are starting values, not a release: the tool manufacturer's data for the specific grade, coating and geometry always takes precedence.
Worked example
Example turning an S235 shaft of Ø 60 mm, coated carbide: With vc = 200 m/min the spindle speed is n = 200·1000/(π·60) = 1061 rpm. With a feed f = 0.3 mm the feed rate is vf = 0.3·1061 = 318 mm/min. With a depth of cut ap = 2.5 mm the material removal rate is Q = 2.5·0.3·200 = 150 cm³/min.
For a turning length of 120 mm with 2 mm approach and overtravel each, L = 124 mm and the machining time t_h = 124/318 = 0.39 min, about 23 seconds per pass. Adding the cutting force for 42CrMo4 (kc1.1 = 2500 N/mm², mc = 0.26) at ap = 3 mm, f = 0.3 mm and κ = 90° gives kc = 3419 N/mm², Fc = 3077 N and a cutting power Pc = 7.7 kW.
Frequently asked questions
How do I calculate the cutting speed?
From diameter and spindle speed: vc = π·d·n/1000 in m/min, with d in mm and n in rpm. The usual route is the reverse one: you look up the cutting speed for the pairing of workpiece material and cutting tool material and derive the spindle speed n = vc·1000/(π·d). The governing diameter is the one being cut, so the workpiece diameter for turning and the tool diameter for milling and drilling. The calculator handles both directions via the vc/n switch.
How do I calculate the feed?
For turning and drilling vf = f·n applies, with the feed per revolution f in mm; for milling vf = fz·z·n with the feed per tooth fz and the number of teeth z. The result is the feed rate in mm/min, from which the machining time t_h = L·i/vf follows together with the feed path L and the number of passes i. The calculator shows a reference range for f and fz per material group; for drilling the feed is additionally estimated as a multiple of the drill diameter.
What is the difference between cutting speed and feed rate?
The cutting speed vc describes the motion that removes the chip, measured at the circumference of the cutting diameter in m/min. The feed rate vf describes the advancing motion along the contour in mm/min and is two to three orders of magnitude smaller. vc mainly governs tool life and cutting temperature, vf governs the machining time. They are linked by the spindle speed: vc fixes n, and n times the feed gives vf.
Where do I find a cutting data table for turning, milling and drilling?
Right on this page: below the calculator a cutting speed reference table is given for each operation, with the common material groups and the cutting tool materials carbide and HSS. Stated are the starting value for normal conditions plus the lower and upper limit. The source is Tabellenbuch Metall (Europa-Lehrmittel), chapter 6.6 on machining.
Where do the cutting speed reference values come from?
The vc ranges of the material selection in the calculator are consolidated from several public sources (reference books, manufacturer catalogues, independent calculators) per material group and cutting tool and apply to average conditions. They are deliberately given as ranges because grade, coating, geometry, cooling and machine stability shift the value considerably. The reference table below the calculator is separate from this: it reproduces the values of Tabellenbuch Metall unchanged. The manufacturer's data for the specific tool always takes precedence.
Which diameter should I enter?
For turning it is the workpiece diameter where the cut takes place (for shoulders the current one). For milling and drilling it is the tool diameter. This distinction determines the correct spindle speed, because the cutting speed always applies at the outer cutting diameter.
How accurate is the cutting force after Kienzle?
The Kienzle approach is a proven approximation for the straight main cutting edge. The correction factors for rake angle, cutting speed, wear and chip compression are not active in this calculator. Real forces are typically 20 to 50 percent higher due to tool wear, and the values kc1.1 and mc scatter by about ±20 percent between sources and batches. The values are suitable for design and machine checks, not as measured data.
Why does my calculated spindle speed differ from the machine step?
The calculator outputs the exact target speed from the cutting speed. Older machines only have fixed speed steps. Therefore the nearest step of a preferred-number series is additionally shown as a hint. On the chosen step a slightly different actual cutting speed results.
What does the lead-in path when drilling mean?
The drill point must first fully engage before the full diameter cuts. This lead-in path is l_s = d/(2·tan(σ/2)) and gives about 0.3·d for the standard point angle of 118°. For short holes this accounts for a considerable part of the time; the calculator includes it automatically.
What is the difference between the milling path conventions?
When passing over a surface the cutter must stand clear in front of and behind the workpiece, so the cutter diameter is added to the path. For a closed slot the cutter centre travels one diameter less, so it is subtracted. In direct mode the entered path is taken unchanged as the path of the cutter centre.
Related tools
Cutting Force & Power (Kienzle)
Pro exportDetermine cutting force, power and machining time for turning, milling and drilling with the Kienzle model.
Machining Time Calculator (Turning, Milling, Drilling)
Free reportCalculate machining time for turning, milling and drilling: spindle speed, cutting speed, feed rate and total feed travel from approach, working length and overtravel.
Tapping Drill & Clearance Hole
Pro exportDetermine tapping drill diameters for metric threads per DIN 13 and clearance holes per EN 20273.
Grinding Calculator - Cutting Speed, Q'w, h_eq
Pro exportCalculate grinding cutting data for external cylindrical grinding and surface grinding: cutting speed v_c, speed ratio q, specific material removal rate Q'w and equivalent chip thickness h_eq with a traffic-light guideline rating.