A free tool for machinists and process planners
Spindle speed from cutting speed, feed rate, machining time, cutting force and power by the Kienzle model, surface roughness from feed and nose radius, tool life by Taylor. Every result with its formula and your numbers in it, every table with its source.
Spindle speed, feed rate, removal rate, cutting force and power, time per pass and theoretical roughness from feed and nose radius.
S235JR, S355J2, C15, C45, 11SMn30 · 125-210 HB · kc1 = 1700 N/mm², mc = 0.25
Start: 200-330 roughing, 280-420 finishing
Start: 0.3-0.5 roughing, 0.1-0.25 finishing
95° for a PCLN/DCLN holder, 45° for SSBC, 93° for DDJN
Positive rake lowers the force by about 1% per degree
0 = no limit
0 = do not check
The suggested values are transcribed from the starting-value tables in the Dormer Pramet (2026), Walter (2021, 2025), Kennametal, Korloy and Morse catalogues - the pages are given under each table below. The catalogue of the actual insert or cutter takes precedence, and tool life on the machine has the last word. Force and power come from the Kienzle model with constants per ISO 513 group - accurate to roughly ±20-30%.
How to
Four moves: material, the numbers off the drawing, the machine's limits, the batch. The rest is computed for you - and shown.
The ISO 513 list sets the cutting-force constants and the starting values in every tab. Then diameter, cutting speed, feed, depth - results update as you type, and the Suggest from table button fills in the middle of the catalogue window.
The max spindle speed field checks whether the spindle can reach the computed rpm at all; if not, everything downstream is computed from the real, lower cutting speed. The spindle power field compares the demand with what the machine has.
Show the working step by step opens the formulas with your numbers substituted, in the order they are computed - ready to carry into your own spreadsheet, and so an apprentice sees where the numbers come from.
The Machining time tab takes the parameters from the Turning, Milling and Drilling tabs and adds passes, hole count, setup and batch size. Tool life tells you what every extra 10% of speed costs; Units is for catalogues in SFM and IPR.
Formulas
One relationship, used both ways: from the catalogue into the program, and from the program back to the catalogue.
Cutting speed vc is the speed at which the cutting edge moves over the machined surface, in metres per minute. In practice the inverse formula is the one you need more often, because the cutting speed comes from the catalogue and the spindle speed is the number that goes into the program.
Two consequences of this formula come up in the shop every day. First: a small diameter means a high spindle speed. A 6 mm end mill at 300 m/min wants 15,900 rpm; on a 10,000 rpm spindle the real cutting speed is 188 m/min, and the feed has to be computed from that - computed from the catalogue speed, the feed per tooth comes out half again too high for the rpm you actually have. Second: in facing at constant rpm, vc falls to zero at the axis. Hence constant surface speed (G96) on CNC lathes, which recomputes the rpm continuously - and hence the need for a maximum-rpm clamp (G50), because near the centre G96 would ask for infinity.
Surface speed and cutting speed are the same quantity; older handbooks say the first, ISO 3002 and current textbooks the second. Imperial catalogues give it in SFM (surface feet per minute); 100 SFM is 30.5 m/min.
Cutting speed
vc = π · D · n / 1000 [m/min]
D in mm, n in rpm. In turning D is the workpiece diameter at the cut; in milling and drilling, the tool diameter.
Spindle speed
n = 1000 · vc / (π · D) [rpm]
Example: D = 50 mm, vc = 200 m/min → n = 1000 · 200 / (3.1416 · 50) = 1273 rpm.
When the spindle cannot keep up
vc real = π · D · nmax / 1000
The calculator does this itself once you enter the machine's maximum rpm, and computes feed, time and power from that speed.
Formulas
Three forms of feed, and the most common mistake when carrying parameters from a catalogue into a program.
Turning and drilling
vf = n · f [mm/min]
Spindle speed times feed per revolution f [mm/rev] - the distance the tool travels in one revolution.
Milling
vf = n · z · fz [mm/min]
Spindle speed times number of teeth times feed per tooth. Example: D = 12, z = 4, fz = 0.08 mm, vc = 200 m/min → n = 5305, vf = 5305 · 4 · 0.08 = 1698 mm/min.
Feed per revolution of a cutter
f = z · fz [mm/rev]
What goes under the F address is always vf, the feed rate in mm/min.
Feed per revolution f [mm/rev] is the distance the tool travels in one revolution - the natural quantity for turning and drilling, where one edge (or two symmetrical ones) works through the whole revolution. Feed per tooth fz [mm/tooth] is the distance between the entries of successive teeth - the natural quantity for milling, where a cutter has z teeth and each takes its own chip. Feed rate vf [mm/min] is the speed of the table or the slide. Milling catalogues give fz, turning-insert catalogues give f, drill catalogues give f or, in the American version, IPR. Confusing feed per revolution with feed per tooth on a four-flute cutter is a fourfold error either way: the edge takes a chip so thin that it rubs instead of cutting, or so thick that the cutter breaks on the first entry.
The third parameter is depth of cut ap [mm] - in turning measured on the radius (6 mm of stock on the diameter is ap = 3 mm in one pass or 2 × 1.5 mm), in milling along the cutter axis. Milling also has the radial width of cut ae [mm], measured perpendicular to the axis; the product ap · ae · vf is the metal removal rate Q, and Q together with the specific cutting force gives the power. In side milling with a narrow radial engagement (ae less than half the diameter) the tooth never reaches the full chip thickness fz, because it enters the material at an angle. That is chip thinning; the calculator computes the mean thickness hm from the engagement angle and tells you how far to raise fz to restore the intended chip. At ae = 10% of D the correction is 1.67 - which is why HSM strategies with narrow stepovers run feeds that look like a typo at first sight.
Tables
A starting point, not an optimum: windows transcribed from manufacturers' catalogues, with page numbers under every table. Material groups per ISO 513 - the same list feeds the suggestions in the calculator.
Every manufacturer prints its own window for its own carbide grade and coating, and the width of that window is exactly so that the process planner can move within it according to fixturing rigidity, coolant, and whether cycle time or tool life matters more. Choosing between the ends is easy to remember: cutting speed mostly decides tool life, feed decides roughness and force, depth decides power and the number of passes. Short of power, lower ap; short of tool life, lower vc; short of surface finish, lower f or take a larger nose radius. Lowering everything at once is the most expensive way to feel safe.
| ISO group | Material | vc roughing [m/min] | vc finishing [m/min] | f roughing [mm/rev] | f finishing [mm/rev] |
|---|---|---|---|---|---|
| P | Unalloyed steel S235JR, S355J2, C15, C45, 11SMn30 | 200-330 | 280-420 | 0.3-0.5 | 0.1-0.25 |
| P | Low-alloy steel (normalised) 16MnCr5, 42CrMo4 (N), 34CrNiMo6, 20MnCr5 | 170-290 | 240-360 | 0.3-0.5 | 0.1-0.25 |
| P | Quenched and tempered and high-alloy steel 42CrMo4 (QT), 1.2312, 1.2344 (+A), X40CrMoV5-1 | 120-200 | 160-260 | 0.25-0.4 | 0.1-0.2 |
| M | Austenitic stainless steel 1.4301 (304), 1.4307 (304L), 1.4404 (316L), 1.4541 | 130-220 | 175-270 | 0.2-0.4 | 0.1-0.2 |
| M | Duplex stainless steel 1.4462 (2205), 1.4410 (2507) | 90-150 | 120-185 | 0.2-0.35 | 0.1-0.18 |
| K | Grey cast iron EN-GJL-200, EN-GJL-250, EN-GJL-300 | 200-340 | 260-410 | 0.3-0.5 | 0.15-0.3 |
| K | Nodular cast iron EN-GJS-400-15, EN-GJS-500-7, EN-GJS-600-3 | 180-300 | 230-370 | 0.25-0.5 | 0.12-0.25 |
| N | Wrought aluminium alloys EN AW-6082 (PA4), EN AW-6061, EN AW-7075 (PA9), EN AW-5083 | 300-800 | 400-1,000 | 0.2-0.5 | 0.1-0.3 |
| N | Cast Al-Si alloys EN AC-AlSi9Cu3, EN AC-AlSi10Mg, EN AC-AlSi12 | 200-500 | 250-600 | 0.2-0.4 | 0.1-0.3 |
| N | Free-cutting brass CuZn39Pb3 (MO58), CuZn40Pb2, CuZn36Pb3 | 250-500 | 320-600 | 0.2-0.4 | 0.08-0.25 |
| N | Copper and lead-free bronzes Cu-ETP, CuSn8, CuAl10Ni5Fe4 | 150-300 | 200-350 | 0.15-0.35 | 0.08-0.2 |
| S | Titanium alloys Ti-6Al-4V (Grade 5), Ti-6Al-4V ELI (Grade 23) | 35-60 | 45-70 | 0.15-0.3 | 0.08-0.2 |
| S | Nickel superalloys Inconel 718, Inconel 625, Hastelloy C-276 | 25-45 | 35-60 | 0.15-0.25 | 0.08-0.15 |
| H | Hardened steel 50-55 HRC 1.2379 (H), 1.2344 (H), 100Cr6 (H), 42CrMo4 (H) | 90-150 | 120-220 | 0.1-0.3 | 0.05-0.15 |
Sources: Dormer Pramet, New Products 2026 (brochure): solid carbide drills RC403/RS403 pp. 10-22 and feed chart p. 24, turning inserts T5405/T9425 pp. 59-127, solid end mills S9xx pp. 150-161 and feed chart p. 162 (P, M, K and S columns of grades T9425 and T5405); Korloy, ISO turning inserts catalogue (extract): uncoated grades H01/H05 p. A18, cBN p. A47, aluminium and copper p. B90 (aluminium, copper, titanium, hardened steel with cBN). The low-alloy, quenched-and-tempered, duplex, nodular-iron and nickel-alloy rows are scaled from the neighbouring column of the same catalogue in the proportion its drill or end-mill table gives, because Dormer prints one column per ISO group. Depth of cut: roughing 2-6 mm, finishing 0.3-1 mm; hardened steel with cBN, ap 0.05-0.5 mm.
| ISO group | Material | vc [m/min] | D6 | D8 | D10 | D12 | D16 | D20 |
|---|---|---|---|---|---|---|---|---|
| P | Unalloyed steel | 90-180 | 0.03 | 0.04 | 0.05 | 0.06 | 0.08 | 0.1 |
| P | Low-alloy steel (normalised) | 90-180 | 0.03 | 0.04 | 0.05 | 0.06 | 0.08 | 0.1 |
| P | Quenched and tempered and high-alloy steel | 60-130 | 0.024 | 0.032 | 0.04 | 0.048 | 0.064 | 0.08 |
| M | Austenitic stainless steel | 60-140 | 0.027 | 0.036 | 0.045 | 0.054 | 0.072 | 0.09 |
| M | Duplex stainless steel | 40-80 | 0.024 | 0.032 | 0.04 | 0.048 | 0.064 | 0.08 |
| K | Grey cast iron | 100-210 | 0.042 | 0.056 | 0.07 | 0.084 | 0.112 | 0.14 |
| K | Nodular cast iron | 90-210 | 0.036 | 0.048 | 0.06 | 0.072 | 0.096 | 0.12 |
| N | Wrought aluminium alloys | 200-600 | 0.039 | 0.052 | 0.065 | 0.078 | 0.104 | 0.13 |
| N | Cast Al-Si alloys | 150-400 | 0.036 | 0.048 | 0.06 | 0.072 | 0.096 | 0.12 |
| N | Free-cutting brass | 90-200 | 0.036 | 0.048 | 0.06 | 0.072 | 0.096 | 0.12 |
| N | Copper and lead-free bronzes | 100-160 | 0.033 | 0.044 | 0.055 | 0.066 | 0.088 | 0.11 |
| S | Titanium alloys | 30-75 | 0.018 | 0.024 | 0.03 | 0.036 | 0.048 | 0.06 |
| S | Nickel superalloys | 20-50 | 0.015 | 0.02 | 0.025 | 0.03 | 0.04 | 0.05 |
| H | Hardened steel 50-55 HRC | 40-120 | 0.015 | 0.02 | 0.025 | 0.03 | 0.04 | 0.05 |
Sources: Walter, Perform line catalogue (2021): DC150 solid carbide drills p. 38, DA110 HSS drills (DIN 338) p. 40, VRR feed chart p. 41, TC115 HSS-E taps p. 58, MC232 solid end mills p. 70 (MC232: vc at ae/D = 1/1, 1/2 and 1/10, hence the width of the window); Dormer Pramet, New Products 2026 (brochure): solid carbide drills RC403/RS403 pp. 10-22 and feed chart p. 24, turning inserts T5405/T9425 pp. 59-127, solid end mills S9xx pp. 150-161 and feed chart p. 162; Kennametal, Recommended Starting Speeds and Feeds - solid carbide end mills, pp. C35-C40 (groups by hardness, fz by diameter) (the only one of the three that lists hardened steel, Inconel and aluminium). fz transcribed from both catalogues' feed charts at D = 10 mm and scaled with diameter: 0.4-0.5% of D for steel, 0.65-0.7% of D for cast iron and aluminium, 0.25-0.3% of D for titanium, superalloys and hardened steel. Indexable cutters take 2-4 times the fz, set by the insert rather than the diameter.
| ISO group | Material | vc carbide [m/min] | vc HSS [m/min] | f D5 carbide | f D8 carbide | f D10 carbide | f D12 carbide | f D16 carbide | f D10 HSS |
|---|---|---|---|---|---|---|---|---|---|
| P | Unalloyed steel | 100-140 | 25-30 | 0.15 | 0.24 | 0.3 | 0.36 | 0.45 | 0.21 |
| P | Low-alloy steel (normalised) | 85-120 | 23-29 | 0.15 | 0.24 | 0.3 | 0.36 | 0.45 | 0.21 |
| P | Quenched and tempered and high-alloy steel | 60-100 | 12-15 | 0.11 | 0.18 | 0.22 | 0.26 | 0.35 | 0.19 |
| M | Austenitic stainless steel | 40-105 | 5-8 | 0.08 | 0.13 | 0.16 | 0.19 | 0.26 | 0.09 |
| M | Duplex stainless steel | 32-85 | - | 0.06 | 0.1 | 0.12 | 0.14 | 0.19 | - |
| K | Grey cast iron | 88-110 | 22-28 | 0.17 | 0.27 | 0.34 | 0.41 | 0.45 | 0.28 |
| K | Nodular cast iron | 71-110 | 17-25 | 0.17 | 0.27 | 0.34 | 0.41 | 0.45 | 0.28 |
| N | Wrought aluminium alloys | 280-400 | 60-90 | 0.17 | 0.27 | 0.34 | 0.41 | 0.45 | 0.24 |
| N | Cast Al-Si alloys | 200-300 | 40-60 | 0.17 | 0.27 | 0.34 | 0.41 | 0.45 | 0.24 |
| N | Free-cutting brass | 160-180 | 41-51 | 0.15 | 0.24 | 0.3 | 0.36 | 0.45 | 0.28 |
| N | Copper and lead-free bronzes | 160-185 | 35-41 | 0.1 | 0.15 | 0.19 | 0.23 | 0.3 | 0.12 |
| S | Titanium alloys | 25-45 | - | 0.08 | 0.12 | 0.15 | 0.18 | 0.24 | - |
| S | Nickel superalloys | 11-40 | 3-4 | 0.05 | 0.08 | 0.1 | 0.12 | 0.16 | 0.07 |
| H | Hardened steel 50-55 HRC | 20-40 | - | 0.05 | 0.06 | 0.08 | 0.1 | 0.13 | - |
Sources: Dormer Pramet, New Products 2026 (brochure): solid carbide drills RC403/RS403 pp. 10-22 and feed chart p. 24, turning inserts T5405/T9425 pp. 59-127, solid end mills S9xx pp. 150-161 and feed chart p. 162 (solid carbide drills 3-5 × D, feeds by alpha code); Walter, Perform line catalogue (2021): DC150 solid carbide drills p. 38, DA110 HSS drills (DIN 338) p. 40, VRR feed chart p. 41, TC115 HSS-E taps p. 58, MC232 solid end mills p. 70 (DC150 carbide and DA110 HSS by machining group P1-S10, feeds by the VRR chart). Where the two catalogues disagree the window covers both - in austenitic stainless Dormer gives 105 m/min, Walter 40. A dash: neither catalogue lists an HSS drill for that group; Machinery's Handbook, 31st ed.: HSS drilling speeds in aluminium alloys (aluminium). Hardened steel: the low end of Kennametal's milling band, because no catalogue at hand prints a drilling table for 50-55 HRC. Holes deeper than 3 × D: peck drilling or through-tool coolant, with feed reduced by 10-20%.
A tap has no feed to choose: in one revolution it must advance exactly one pitch, so vf = n · P. What is left to choose is the cutting speed and the tap drill. For coated HSS-E taps Walter Prototyp TC115 gives (thread depth 1.5-2.5 × D): unalloyed and low-alloy steel 26-37 m/min, quenched and tempered 9-14, austenitic stainless 6-8, duplex 4-6, grey cast iron 32-44, nodular 9-22, hardened wrought aluminium 22-32, brass 25-48, titanium 4-8, nickel alloys 3; Morse for HSS taps: steel under 25 HRC 10-40, stainless 5-15, cast iron 8-35, titanium 6-10, Inconel 4-8. For coarse metric threads the rule is D − P, and the standard rounds it to a drill that exists.
| Thread | Pitch P [mm] | Tap drill [mm] | D − P [mm] | n at vc = 10 m/min | vf [mm/min] |
|---|---|---|---|---|---|
| M3 | 0.5 | 2.5 | 2.5 | 1,061 | 531 |
| M4 | 0.7 | 3.3 | 3.3 | 796 | 557 |
| M5 | 0.8 | 4.2 | 4.2 | 637 | 509 |
| M6 | 1 | 5 | 5 | 531 | 531 |
| M8 | 1.25 | 6.8 | 6.75 | 398 | 497 |
| M10 | 1.5 | 8.5 | 8.5 | 318 | 477 |
| M12 | 1.75 | 10.2 | 10.25 | 265 | 464 |
| M14 | 2 | 12 | 12 | 227 | 455 |
| M16 | 2 | 14 | 14 | 199 | 398 |
| M18 | 2.5 | 15.5 | 15.5 | 177 | 442 |
| M20 | 2.5 | 17.5 | 17.5 | 159 | 398 |
| M22 | 2.5 | 19.5 | 19.5 | 145 | 362 |
| M24 | 3 | 21 | 21 | 133 | 398 |
| M27 | 3 | 24 | 24 | 118 | 354 |
| M30 | 3.5 | 26.5 | 26.5 | 106 | 371 |
| M36 | 4 | 32 | 32 | 88 | 354 |
Pitches per ISO 261 / ISO 724, tap drills per DIN 336 (recommended sizes, about 75-80% thread height). Tapping speeds in the calculator: Walter, Perform line catalogue (2021): DC150 solid carbide drills p. 38, DA110 HSS drills (DIN 338) p. 40, VRR feed chart p. 41, TC115 HSS-E taps p. 58, MC232 solid end mills p. 70 (TC115) and Morse, HSS taps catalogue 2021, pp. 110-119. In ductile materials a drill 0.1 mm larger lowers the torque on the tap with no meaningful loss of thread strength.
Time
Cutting time is the tool's path through the material divided by the feed rate. The whole difficulty is getting the path right.
Turning time
tm = L / (n · f) [min]
L is the turned length plus approach (1-2 mm) and overrun. A Ø50 shaft, L = 100 mm, 1273 rpm, f = 0.25: 100 / (1273 · 0.25) = 0.31 min, or 19 s per pass. 6 mm of stock on the diameter at ap = 2 mm is two passes: ⌈(6/2) / 2⌉.
Milling time
tm = (L + la + lu) / vf [min]
Approach la: D/2 when the cutter is buried past its centre, √(ae · (D − ae)) when shallower; overrun the same. For pocket roughing the volume method is more accurate: time = V / Q, Q = ap · ae · vf / 1000 [cm³/min].
Drilling time
tm = (l + point + overrun) / (n · f) [min]
Drill point length: (D/2) / tan(σ/2) - 0.30 · D for a 118° point, 0.18 · D for 140°. A through hole also needs an overrun. With many holes, positioning (2-3 s per hole) takes more time than the drilling itself.
The Machining time tab computes milling by volume - you enter the volume to remove, and Q comes from the parameters in the Milling tab. This ignores the moves between passes, so it underestimates small pockets and thin ribs; for large volumes it is accurate to a few percent. Peck cycles (G83) are not modelled - at 5 × D add 30-50% to the time.
Cutting time is usually 40-70% of cycle time. The rest is tool changes (3-8 s each on a machining centre, 1-2 s on a turret lathe), rapid moves, in-cycle probing, door opening and part exchange. The price of the part also carries the setup time spread over the batch and the material cost - how those add up to a machine-hour rate, and how an automated quote computes the same thing from the customer's file, is described on the page about instant CNC quoting.
The Kienzle model
One equation from 1952 that every catalogue still uses.
Cutting force is proportional to the cross-section of the cut layer, but the constant of proportionality is not constant: the thinner the chip, the more energy per unit volume goes into deformation and friction at the edge. Otto Kienzle put that into one equation in which the specific cutting force kc rises as the chip thickness falls.
What it is for: the cutting power has to be compared with the spindle power divided by the drive efficiency (0.75-0.85), and the torque with the spindle characteristic, because below its rated speed a spindle has constant torque, not constant power. A roughing pass in 42CrMo4 at ap = 4 mm and f = 0.4 mm/rev needs about 12 kW; on a lathe with a 7.5 kW spindle it can only be done in two passes or at a lower feed. The calculator shows this as a warning once you enter the machine's power.
Specific cutting force
kc = kc1 · h−mc · (1 − γ0/100)
kc [N/mm²], h - chip thickness [mm], kc1 - specific force at h = 1 mm, mc - material exponent (0.2-0.3). The term (1 − γ0/100) is the catalogue correction for rake angle: about 1% of force per degree.
Force, power, torque
Fc = kc · ap · f [N]
Pc = Fc · vc / 60,000 [kW]
Mc = Pc · 30,000 / (π · n) [Nm]
Turning: h = f · sin κr, cross-section = ap · f. Milling: kc is evaluated at the mean chip thickness hm and the power from the removal rate Q. Drilling: h = (f/2) · sin(σ/2), because each of the two lips takes half the feed.
| ISO group | Material | Hardness | kc1 [N/mm²] | mc |
|---|---|---|---|---|
| P | Unalloyed steel (P1.1 / P1.2) | 125-210 HB | 1,700 | 0.25 |
| P | Low-alloy steel (normalised) (P2.1 / P2.2) | 175-240 HB | 1,950 | 0.25 |
| P | Quenched and tempered and high-alloy steel (P2.5 / P3.0) | 260-330 HB | 2,200 | 0.25 |
| M | Austenitic stainless steel (M1.0) | 200-300 HB | 2,000 | 0.21 |
| M | Duplex stainless steel (M3.2) | 230-260 HB | 2,300 | 0.21 |
| K | Grey cast iron (K2.2) | 180-245 HB | 1,100 | 0.28 |
| K | Nodular cast iron (K3.2 / K3.3) | 215-265 HB | 1,300 | 0.28 |
| N | Wrought aluminium alloys (N1.2) | 60-100 HB | 600 | 0.25 |
| N | Cast Al-Si alloys (N1.3) | 75-90 HB | 650 | 0.25 |
| N | Free-cutting brass (N3.2) | 90 HB | 550 | 0.25 |
| N | Copper and lead-free bronzes (N3.1) | 100 HB | 1,350 | 0.25 |
| S | Titanium alloys (S4.3) | 330-375 HB | 1,400 | 0.23 |
| S | Nickel superalloys (S2.0) | 250-350 HB | 2,800 | 0.25 |
| H | Hardened steel 50-55 HRC (H1.1 / H1.2) | 50-55 HRC | 3,400 | 0.25 |
Representative values per sub-group from two independent tables: Sandvik Coromant, workpiece materials (kc1 at h = 1 mm, mc, by ISO 513 sub-group) and Walter, Technical Compendium General 2025, p. F9 (kc1.1 and mc by machining group) - for every group the value lies within both (unalloyed steel: Sandvik 1500-1820, Walter 1500-1700; grey cast iron: Sandvik 1100, Walter 800-1200; nickel alloys: Sandvik 2650-3000, Walter 2800-3000). Rake angle 0°. The same steel in a different heat-treatment condition differs by 10-20%, which is why the result should be read as a ±20-30% estimate.
Surface finish
Theoretical roughness
Rt = f² / (8 · rε)
Ra ≈ f² / (31.2 · rε)
f and rε in mm, result in mm (times 1000 for µm). Example: f = 0.2 mm, rε = 0.8 mm → Ra = 1.6 µm, Rt = 6.25 µm - which is why so many finishing inserts are run at 0.2 / 0.8.
Turning with a nose of radius rε leaves arc-shaped grooves on the surface, spaced one feed apart; their geometric height and arithmetic mean follow from the kinematics alone. That is the theoretical roughness, a lower bound: the real value is higher by built-up edge, vibration, edge wear and the elastic recovery of the material at very small feeds. The practical rule: to reach the Ra on the drawing, aim one class lower on the formula.
The formula earns its keep the other way round - it shows that roughness grows with the square of the feed, so half the feed gives four times the finish, while twice the nose radius gives only twice. In face milling the same role is played by feed per revolution and a wiper insert.
Taylor's equation
Taylor, 1907
vc · Tn = C
T - tool life [min], C - a constant (the speed that gives a life of 1 min), n - an exponent set mainly by the tool material. Catalogue cutting speeds are usually quoted for T = 15 min.
| Tool material | n (mid-range) | Range in the literature | +10% vc means a tool life of |
|---|---|---|---|
| HSS / HSS-E | 0.12 | 0.08-0.20 | −55% |
| Uncoated carbide | 0.25 | 0.20-0.50 | −32% |
| Coated carbide | 0.35 | 0.20-0.50 | −24% |
| Ceramics | 0.55 | 0.50-0.70 | −16% |
Ranges per Kalpakjian and Schmid (Manufacturing Engineering and Technology); an exponent from your own tool-life test per ISO 3685 always beats the table.
After twenty-six years of trials and several hundred tons of machined steel, Frederick Taylor put the dependence of tool life on cutting speed into one equation, and its practical content is in the exponent. At n = 0.12 (HSS) a 10% increase in speed cuts tool life by more than half; at n = 0.35 (coated carbide) by about a quarter. That is why it never pays to speed up HSS, and sometimes pays to speed up carbide - when a machine minute is expensive and an insert is cheap. The calculator works both ways: the speed that gives a required life, and the life left after speeding up.
Bibliography
The formulas come from the textbooks, the Kienzle constants from two independent manufacturers' tables, and the speed and feed windows from the starting-value tables in the catalogues named under each table, with page numbers. Where catalogues disagree the window spans both; where none gives a value the table shows a dash rather than a number. A few turning rows are scaled from the neighbouring column of the same catalogue and the table says which. Where sources differ among themselves (Kienzle constants for the same grade can differ by 15%), a value lying within both was taken.
Found an error in a formula, or a value that disagrees with your catalogue? Write to us - we will fix it and add the source. metronq.com/en/cutting-parameters-calculator
[Kienzle 1952] Kienzle O., Die Bestimmung von Kräften und Leistungen an spanenden Werkzeugen und Werkzeugmaschinen, VDI-Z 94 (1952), pp. 299-305. The source of the specific cutting force model kc = kc1 · h^(−mc).
[Taylor 1907] Taylor F. W., On the Art of Cutting Metals, Transactions of the ASME 28 (1907). The tool-life equation vc · T^n = C.
[Grzesik 2018] Grzesik W., Podstawy skrawania materiałów konstrukcyjnych (Fundamentals of machining engineering materials), 3rd ed., PWN, Warsaw 2018, ISBN 978-83-01-19919-7. Cut-layer geometry, theoretical roughness, parameter selection.
[Jemielniak 2018] Jemielniak K., Obróbka skrawaniem. Podstawy, dynamika, diagnostyka (Machining: fundamentals, dynamics, diagnostics), Warsaw University of Technology Press, 2018, ISBN 978-83-7814-860-9. Kinematics of turning and milling, cutting forces.
[Klocke 2011] Klocke F., Manufacturing Processes 1: Cutting, Springer, Berlin 2011, ISBN 978-3-642-11978-1. The Kienzle model, chip thickness in milling, tool life.
[Sandvik] Sandvik Coromant, Metal Cutting Technology - Training Handbook, and Machining formulas and definitions: turning, milling, drilling - the power, torque and mean chip thickness formulas; the kc1 and mc table by ISO 513 group (workpiece materials). publisher's site
[Dormer Pramet 2026] Dormer Pramet, New Products 2026 (brochure): starting vc by ISO 513 sub-group for solid carbide drills RC403/RS403 (pp. 10-22) with the feed chart (p. 24), turning inserts T5405 and T9425 in P/M/K/S columns (pp. 59-127) and solid end mills S9xx (pp. 150-161) with the feed-per-tooth chart (p. 162). publisher's site
[Walter 2021] Walter, Perform line catalogue (2021): DC150 solid carbide (p. 38) and DA110 HSS DIN 338 drills (p. 40) by machining group P1-H4, the VRR feed chart (p. 41), Walter Prototyp TC115 HSS-E taps (p. 58), MC232 solid end mills by ae/D (p. 70). publisher's site
[Walter 2025] Walter, Technical Compendium General 2025, p. F9: specific cutting force kc1.1 and exponent mc by Walter machining group - a second source of Kienzle constants, independent of Sandvik's.
[Kennametal] Kennametal, Recommended Starting Speeds and Feeds - solid carbide end mills (pp. C35-C40): vc and fz by diameter for steels by hardness, stainless steels, cast iron, titanium, nickel alloys, aluminium and hardened steel 51-60 HRC.
[Korloy] Korloy, ISO turning inserts catalogue (extract): recommended cutting speeds of uncoated grades H01/H05 (p. A18), cBN inserts for hardened steel (p. A47), aluminium and copper alloys with kc and feed (p. B90).
[Morse 2021] Morse, HSS and HSS-Co taps catalogue (2021), pp. 110-119: machine-tap cutting speeds by material (steel, stainless, cast iron, titanium, Inconel, hardened steel).
[Machinery's Handbook] Oberg E., Jones F. D., Horton H. L., Ryffel H. H., Machinery's Handbook, 31st ed., Industrial Press, New York 2020. Milling approach and overrun, roughness from feed and nose radius, thread tables, HSS drilling speeds.
[Kalpakjian 2020] Kalpakjian S., Schmid S. R., Manufacturing Engineering and Technology, 8th ed., Pearson 2020. Ranges of the Taylor exponent for HSS, carbides and ceramics.
[Standards] ISO 3002-1 (basic quantities in cutting: vc, f, ap, κr), ISO 513:2012 (material groups P, M, K, N, S, H), ISO 3685:1993 (tool-life testing), ISO 261 and ISO 724 (metric threads - profile and pitches), ISO 21920-2:2021 (roughness parameters Ra, Rz, Rt; replaced the withdrawn ISO 4287).
[Cichosz 2006] Cichosz P., Narzędzia skrawające (Cutting tools), WNT, Warsaw 2006. Edge geometry, entering and rake angles, tool materials.
FAQ
Read on in the blog:
From n = 1000 · vc / (π · D), where vc is the cutting speed in m/min and D the diameter in mm - the workpiece in turning, the tool in milling and drilling. For D = 50 mm and vc = 200 m/min: n = 1000 · 200 / (3.1416 · 50) = 1273 rpm. If the spindle cannot reach that, the real cutting speed drops and the feed rate with it - the calculator handles this once you enter the machine's maximum rpm.
In turning and drilling vf = n · f (rpm times feed per revolution). In milling vf = n · z · fz, rpm times number of teeth times feed per tooth. A D = 12 mm cutter with z = 4 and fz = 0.08 mm at 5300 rpm gives vf = 5300 · 4 · 0.08 = 1696 mm/min. That is the value that goes into the program as F.
vc = π · D · n / 1000 [m/min]. Diameter D in mm, spindle speed n in rpm. It works both ways: from the rpm in a program you can check what cutting speed the edge is actually running at. In facing at constant rpm vc falls towards the axis, which is why CNC lathes have constant surface speed (G96).
Yes - the same quantity, vc, in m/min or SFM. Older handbooks and some catalogues say surface speed; ISO 3002 and current textbooks say cutting speed. 1 SFM = 0.3048 m/min.
Cutting time is the tool path divided by the feed rate: tm = L / vf. In turning tm = L / (n · f); with several passes multiply by their number - 6 mm of stock on the diameter at ap = 2 mm is 2 passes (3 mm on the radius). In milling add the approach and overrun to the length; in drilling add the drill point (0.3 · D for a 118° point). The Machining time tab adds it all up from the parameters in the other tabs.
The rule for coarse metric threads: drill diameter = D − P (nominal diameter minus pitch). M6 x 1 → 5.0 mm; M8 x 1.25 → 6.8 mm; M10 x 1.5 → 8.5 mm; M12 x 1.75 → 10.2 mm. The table in the calculator lists the standard sizes from M3 to M36. In ductile materials (aluminium, stainless) a drill 0.1 mm larger lowers the torque on the tap without losing thread strength.
From the catalogue starting-value tables for coated carbide inserts (Dormer Pramet 2026, Korloy): unalloyed steel 200-330 m/min roughing and 280-420 finishing, austenitic stainless 130-220 and 175-270, grey cast iron 200-340 and 260-410, wrought aluminium 300-1000 (usually limited by the spindle), titanium 35-70, nickel alloys 25-60, hardened steel 50-55 HRC with cBN 90-220. HSS drills run at 5-30 m/min, HSS-E taps at 3-48 depending on the material. These are starting values - the insert's own catalogue takes precedence and tool life has the last word.
From the Kienzle model: specific cutting force kc = kc1 · h^(−mc), where h is the chip thickness and kc1 and mc are material constants (about 1700 N/mm² at mc = 0.25 for C45 steel). Cutting force is kc times the cut cross-section, power is force times cutting speed. kc1 and mc are taken from published manufacturers' tables by ISO 513 group, so the result is a ±20-30% estimate - enough to check whether the spindle can take the pass.
Yes. When the radial width of cut ae is less than half the cutter diameter, the tooth never reaches the full chip thickness fz. The calculator computes the mean thickness hm and the maximum hex from the engagement angle and gives a corrected feed per tooth that restores the intended chip thickness - the standard correction for HSM with narrow stepovers.
The cutting time from the calculator is one component. The price also needs the non-cutting times, setup, material with stock allowance and the machine-hour rate. MetronQ does exactly that from the customer's file - a 3D model or a drawing: it measures the geometry, picks the operations, computes the times and prices them at the shop's rates, and a process planner approves the result.
Everything this page computes feeds one number the customer cares about: the price of the part. MetronQ computes it from the customer's file - a 3D model or a drawing - measures the geometry, picks the operations for the shop's machines, computes the times and prices them at rates the shop calibrates itself. A process planner approves, the customer has a quote in minutes.
