Worked examples
- Lathe: turning C45 steel at Ø50 mm and 200 m/min → n = 1000 × 200 / (π × 50) ≈ 1,273 RPM.
- Mill: Ø10 mm end mill in steel at 120 m/min → n = 1000 × 120 / (π × 10) ≈ 3,820 RPM.
- The other way round: an Ø8 mm drill at 2,000 RPM runs at π × 8 × 2,000 / 1000 ≈ 50 m/min.
Cutting speed chart by material
Starting values for coated carbide tools and a medium cut, the same ones the site's calculator uses. For high-speed steel (HSS), use about one third. Adjust them with the tool maker's data and the condition of your machine.
| Material | ISO | Turning Vc (m/min) | Milling Vc (m/min) | Drilling Vc (m/min) |
|---|---|---|---|---|
| Low-carbon steel S235 / St37 | P | 216–378 | 216–378 | 151–284 |
| Medium-carbon steel C45 / 1045 | P | 194–302 | 194–302 | 136–227 |
| Alloy steel 42CrMo4 / 4140 | P | 162–259 | 162–259 | 113–194 |
| Austenitic stainless 304 / 1.4301 | M | 130–216 | 76–130 | 91–162 |
| Austenitic stainless 316 / 1.4401 | M | 108–194 | 65–108 | 76–146 |
| Gray cast iron GG25 / EN-GJL-250 | K | 162–270 | 162–270 | 113–203 |
| Aluminum 6082 / AlMgSi1 | N | 432–1,080 | 270–648 | 302–810 |
| Aluminum 7075 / AlZnMgCu | N | 378–972 | 238–594 | 265–729 |
| Brass CuZn39Pb3 | N | 216–540 | 216–540 | 151–405 |
| POM-C / Delrin plastic | N | 270–540 | 270–540 | 86–216 |
| Titanium Ti6Al4V | S | 43–86 | 43–86 | 30–65 |
| Inconel 718 | S | 22–54 | 27–38 | 15–41 |
| Hardened steel 50-55 HRC | H | 86–162 | 86–162 | 60–122 |
01On a lathe, the diameter is the workpiece's
In turning, D is the workpiece diameter at the cutting point, not the tool's. That is why facing towards the centre lowers Vc even if RPM stays the same. To keep it constant, lathes use G96 (constant surface speed) with a spindle limit (G50 or G92 S depending on the control), which stops the chuck from over-speeding at the centre.
02On mills and drills, the diameter is the tool's
In milling and drilling, D is the cutter or drill diameter. A small cutter needs high RPM to reach the same Vc: if the machine cannot get there, run at maximum RPM and adjust feed per tooth, not the other way round.
03What cutting speed depends on
Mainly the workpiece material (aluminium takes far more Vc than stainless steel or titanium) and the tool material (coated carbide handles about three times more than HSS). Coolant, machine and workholding rigidity, and roughing versus finishing also matter. More Vc means more output, but a shorter tool life.
04Signs that Vc is wrong
Too high: the edge wears quickly, changes colour, chips come out blue or burnt and the insert shows crater wear. Too low: built-up edge (material sticks, typical in aluminium and mild steel), poor finish and chips that do not break. If wear is fast, lower Vc first; if there is built-up edge, raise it.
05Common mistakes
Using the tool diameter on a lathe, mixing m/min with surface feet per minute, forgetting the spindle limit with G96 and taking a catalogue Vc without checking whether it is for HSS or carbide. Always check that the resulting RPM fits the machine.
Frequently asked questions
What is cutting speed?
It is how fast the cutting edge moves across the material, in m/min. It depends on the workpiece and tool materials, and RPM is calculated from it: n = 1000 × Vc / (π × D).
What is the difference between cutting speed and RPM?
Vc is the edge speed over the material (m/min) and is chosen by material; RPM is spindle revolutions and depends on Vc and diameter. For the same Vc, a smaller diameter needs more RPM.
What cutting speed is used for steel?
For a carbon steel such as C45 with coated carbide, about 190-300 m/min for turning and milling as a starting point; with HSS, about one third. The chart on this page lists values by material.
What is G96?
It is constant surface speed on a lathe: the control changes RPM with the diameter to keep Vc. It is always used with a spindle limit (G50 or G92 S, depending on the control).
Indicative starting values. Confirm them with the tool maker's data, the actual material and your machine's rigidity. Last updated: