Most tool failures trace back to parameters chosen by feel rather than calculation. The arithmetic is simple, and getting it right is the difference between a tool that lasts an afternoon and one that lasts a week.
The Four Numbers
- Cutting speed (Vc), in m/min — how fast the cutting edge passes through the material. A property of the material and tool, not the machine.
- Spindle speed (n), in RPM — what you actually program.
- Feed per tooth (fz), in mm — how much material each flute removes per revolution.
- Feed rate (Vf), in mm/min — what the machine moves at.
The Two Formulas
Convert cutting speed to spindle speed:
n = (Vc × 1000) ÷ (π × D) where D is the tool diameter in mm.
Convert feed per tooth to feed rate:
Vf = n × fz × z where z is the number of flutes.
Example: a 10 mm 4-flute end mill in mild steel at Vc = 120 m/min and fz = 0.05 mm.
n = (120 × 1000) ÷ (3.1416 × 10) = 3820 RPM
Vf = 3820 × 0.05 × 4 = 764 mm/min
Starting Cutting Speeds for Coated Carbide
| Material | Milling (m/min) | Turning (m/min) | Drilling (m/min) |
|---|---|---|---|
| Aluminium | 400–1000 | 300–800 | 100–250 |
| Mild steel | 120–200 | 200–350 | 60–100 |
| Alloy steel | 80–150 | 150–280 | 40–80 |
| Stainless (304/316) | 80–120 | 120–200 | 25–45 |
| Cast iron | 100–180 | 150–300 | 50–90 |
| Hardened steel HRC50+ | 50–120 | 80–150 | — |
| Titanium | 40–70 | 50–90 | 15–30 |
| Inconel | 20–35 | 25–50 | 8–20 |
Feed per Tooth: The Number That Matters
A rough guide for solid carbide end mills:
| Tool diameter | Steel (mm/tooth) | Aluminium (mm/tooth) |
|---|---|---|
| 3 mm | 0.010–0.020 | 0.020–0.040 |
| 6 mm | 0.025–0.045 | 0.050–0.090 |
| 10 mm | 0.040–0.070 | 0.080–0.150 |
| 16 mm | 0.060–0.110 | 0.120–0.220 |
| 20 mm | 0.080–0.140 | 0.150–0.280 |
The most damaging mistake in this table is going too low. Below a minimum chip thickness the edge stops cutting and starts rubbing — which generates heat, work-hardens the surface and kills the tool far faster than a heavy feed would.
Adjusting From the Starting Point
- Poor tool life? Reduce speed first. Speed drives temperature, and temperature drives wear.
- Poor surface finish? Reduce feed per tooth, or increase the corner radius.
- Chatter? Change speed (up or down) to move away from the resonant frequency; increasing feed often helps too.
- Tool chipping? Reduce feed and improve rigidity.
- Burning or discolouration? Too much speed or not enough feed — check you are not rubbing.
Two Corrections People Forget
Chip thinning. Below 50% radial engagement, increase feed to compensate (see our guide to trochoidal milling).
Effective diameter. With a ball nose tool taking a shallow depth of cut, the actual cutting diameter is much smaller than the tool diameter — so the real cutting speed is much lower than calculated. Use the effective diameter at the depth you are cutting, or you will be running far too slowly.
Every tool we ship comes with recommended starting parameters for the main ISO material groups. Ask our engineers if you would like a parameter sheet for your specific material and machine.
Talk to Our Engineers
MSU Tools manufactures the full range of solid carbide and indexable tooling discussed here. Tell us your material, machine and application and we will recommend the optimal tool, grade and starting parameters — or design a custom tool to your drawing. Send us your requirement for a reply within one business day.
Questions about this topic?
Our engineers are happy to advise on tools, grades and cutting parameters.