Speeds & feeds calculator
Spindle speed and feed for milling, drilling, turning and tapping — from the tool makers' own published cutting data, every number with its source. No sign-up.
How it is calculated
Two numbers come from the tool maker: the cutting speed Vc (metres of edge per minute) and the chip load — fz per tooth for milling, fn per revolution for drilling and turning. The rest is arithmetic:
F = fz · z · n [mm/min] — milling
F = fn · n [mm/min] — drilling, turning
F = P · n [mm/min] — tapping
Worked examples
Milling. A Ø10 carbide end mill, 3 flutes, roughing wrought aluminium. The tool maker's published catalogue data gives Vc 400 m/min and fz 0.070 mm/tooth at Ø10: n = 1000 × 400 / (π × 10) = 12,732 rpm; F = 0.070 × 3 × 12,732 = 2,674 mm/min. If the machine tops out at 8,000 rpm, n is 8,000 and F = 0.070 × 3 × 8,000 = 1,680 mm/min — the chip per tooth stays what the maker asked for.
Drilling. A Ø8 carbide drill in 1045 steel: the tool maker's published catalogue data gives Vc 60 m/min and fn 0.150 mm/rev at Ø8: n = 2,387 rpm, F = 0.150 × 2,387 = 358 mm/min.
Starting values — Ø10 carbide end mill, roughing, 4 flutes
| Material | Vc m/min | fz | S rpm | F mm/min | Source |
|---|---|---|---|---|---|
| Low-carbon / free-cutting steel (1018, S235) | 145 | 0.085 | 4,615 | 1,569 | Tool maker's catalogue data |
| Medium-carbon / alloy steel (1045, 4140) | 105 | 0.082 | 3,342 | 1,096 | Tool maker's catalogue data |
| Tool / die steel, annealed (H13, D2, P20) | 85 | 0.072 | 2,706 | 779 | Tool maker's catalogue data |
| Austenitic stainless (304, 316) | 80 | 0.041 | 2,546 | 418 | Tool maker's catalogue data |
| Duplex / PH stainless (17-4, 2205) | 50 | 0.044 | 1,592 | 280 | Tool maker's catalogue data |
| Martensitic / ferritic stainless (420, 430) | 60 | 0.053 | 1,910 | 405 | Tool maker's catalogue data |
| Grey cast iron | 120 | 0.079 | 3,820 | 1,207 | Tool maker's catalogue data |
| Nodular (ductile) cast iron | 110 | 0.067 | 3,501 | 938 | Tool maker's catalogue data |
| Wrought aluminium (6061, 7075) | 400 | 0.070 | 12,732 | 3,565 | Tool maker's catalogue data |
| Cast / high-silicon aluminium | 180 | 0.058 | 5,730 | 1,329 | Tool maker's catalogue data |
| Titanium (Ti-6Al-4V) | 45 | 0.041 | 1,432 | 235 | Tool maker's catalogue data |
| Nickel alloy (Inconel) | 25 | 0.035 | 796 | 111 | Tool maker's catalogue data |
| Hardened steel 45–55 HRC | 50 | 0.045 | 1,592 | 286 | Tool maker's catalogue data |
| Hardened steel 55–65 HRC | 70 | 0.044 | 2,228 | 392 | Tool maker's catalogue data |
Starting values — Ø8 carbide drill
| Material | Vc m/min | fn | S rpm | F mm/min | Source |
|---|---|---|---|---|---|
| Low-carbon / free-cutting steel (1018, S235) | 70 | 0.130 | 2,785 | 362 | Tool maker's catalogue data |
| Medium-carbon / alloy steel (1045, 4140) | 60 | 0.150 | 2,387 | 358 | Tool maker's catalogue data |
| Tool / die steel, annealed (H13, D2, P20) | 50 | 0.140 | 1,989 | 279 | Tool maker's catalogue data |
| Austenitic stainless (304, 316) | 20 | 0.090 | 796 | 72 | Tool maker's catalogue data |
| Duplex / PH stainless (17-4, 2205) | 20 | 0.090 | 796 | 72 | Tool maker's catalogue data |
| Martensitic / ferritic stainless (420, 430) | 40 | 0.100 | 1,592 | 159 | Tool maker's catalogue data |
| Grey cast iron | 80 | 0.200 | 3,183 | 637 | Tool maker's catalogue data |
| Nodular (ductile) cast iron | 80 | 0.200 | 3,183 | 637 | Tool maker's catalogue data |
| Wrought aluminium (6061, 7075) | 90 | 0.160 | 3,581 | 573 | Tool maker's catalogue data |
| Cast / high-silicon aluminium | 90 | 0.160 | 3,581 | 573 | Tool maker's catalogue data |
| Brass / bronze | 90 | 0.160 | 3,581 | 573 | Tool maker's catalogue data |
| Copper | 90 | 0.160 | 3,581 | 573 | Tool maker's catalogue data |
| Titanium (Ti-6Al-4V) | 10 | 0.070 | 398 | 28 | Tool maker's catalogue data |
| Nickel alloy (Inconel) | 10 | 0.080 | 398 | 32 | Tool maker's catalogue data |
| Hardened steel 45–55 HRC | 10 | 0.070 | 398 | 28 | Tool maker's catalogue data |
| Hardened steel 55–65 HRC | 10 | 0.060 | 398 | 24 | Tool maker's catalogue data |
The low end of each maker's published range, at that diameter. A starting value is where a first cut begins — rigidity, stick-out, coolant and the machine decide where it ends.
Questions
What is the difference between Vc and rpm?
Vc is how fast the cutting edge moves through the material, in metres per minute — it belongs to the tool and the material. rpm is how fast the spindle turns. The same Vc means a high rpm on a small tool and a low one on a big tool: n = 1000·Vc / (π·D).
Why a “starting value”?
Makers publish a range, measured on their own test setups. The calculator starts at the low end. Raise it when the cut is quiet and the chips look right; lower it on a long stick-out, a thin wall or a weak holding.
What is fz, and what is fn?
fz is the chip each tooth takes, in mm — milling. fn is the feed per spindle revolution, in mm — drilling and turning. Feed per minute is fz × teeth × rpm, or fn × rpm.
On a lathe, which number do I program?
With constant surface speed (G96) you program Vc itself and the control changes the rpm as the diameter changes — cap it with G50. The rpm shown is the one at the diameter you typed.
The whole part, not one tool
MEKLYRA reads the STEP and the drawing and plans every setup, tool and cutting value for the part — from your own machine and tools, each number with its source.