How this instrument works
Cutting speed is a property of the material and the tool coating, not the machine — it is the surface distance the cutting edge sweeps past the workpiece per minute, quoted in metres per minute. A spindle turning a small drill and a spindle turning a large face mill can share the same cutting speed while spinning at completely different RPM, because the edge of a wider tool travels farther per revolution. The conversion is circumference-based: n = 1000·Vc ⁄ (π·D). The 1000 simply reconciles metres in Vc with millimetres in the diameter D before the division.
Feed rate answers a separate question: how fast does the table actually move in millimetres per minute? It is built from feed per tooth, fz — the thickness of the chip each individual flute is meant to shave off on its pass — multiplied by the number of flutes Z and by the spindle speed n, since every flute takes one bite per revolution. Vf = n·fz·Z. Get fz from the tool manufacturer's chip-load chart; it depends on the tool material, coating, and the workpiece alloy, not on any physics this calculator can derive for you.
Both formulas assume steady-state, full engagement cutting. They say nothing about spindle torque limits, tool deflection, or the chip-thinning effect that shows up when the radial depth of cut is a small fraction of the tool diameter — in that case the real chip is thinner than fz and the programmed feed per tooth is usually increased to compensate. Treat the two numbers here as the starting point a setup sheet calls for, then adjust from there once the cut is actually running.
- Enter the Cutting speed, m/min for the material and tool coating, taken from a machining data chart or the tool manufacturer's catalog.
- Enter the Tool diameter — the cutter's actual cutting diameter in mm, not the shank diameter.
- Enter the Feed per tooth, mm — the recommended chip load per flute for that tool and material combination.
- Enter the Number of flutes/teeth cut into the tool.
- Read off the Spindle speed, RPM and Feed rate, mm/min and enter both directly into the CNC control.
Worked example — a 10 mm end mill in mild steel
A 10 mm, 4-flute carbide end mill is set up to cut mild steel at a cutting speed of 100 m/min, a reasonable starting figure for that pairing. The RPM comes first: n = 1000 × 100 ⁄ (π × 10) = 3183.09886184, which the readout rounds to about 3,183 RPM — that is the number typed into the spindle-speed line of the setup sheet before the first cut is taken.
With the spindle speed fixed, the feed per tooth for this tool and material is 0.05 mm. Feed rate follows directly: Vf = 3183.09886184 × 0.05 × 4 = 636.619772368 mm/min, roughly 636.6 mm/min. Program the spindle at 3,183 RPM and the feed at 636.6 mm/min and each of the four flutes removes a 0.05 mm chip on every pass, which is the whole point of running the two formulas back to back rather than guessing a feed rate outright.
Questions
Why does spindle speed depend on tool diameter?
Because cutting speed is a surface measurement, not a rotational one. A wider tool's edge covers more distance in one turn than a narrow tool's does, so to hold the same cutting speed the wider tool must turn slower. Halving the diameter roughly doubles the RPM needed for the same Vc, which is why a 20 mm cutter at 100 m/min runs at about 1,592 RPM against a 10 mm cutter's 3,183 RPM.
Where do the cutting speed and feed-per-tooth numbers come from?
From the tool manufacturer's cutting-data tables, not from this instrument. They depend on the tool material and coating, the workpiece alloy and hardness, and the machine's rigidity, and typically come as a range rather than one fixed value. Start near the middle of the recommended range and adjust after watching the chip color and listening to the cut.
What happens if the RPM is set too high or too low?
Too high, and the edge overheats faster than it can shed the heat, which burns the coating and shortens tool life sharply. Too low, and the edge rubs instead of shearing cleanly, which builds up material on the cutting edge and can chip or snap it. Both failure modes trace back to the same spindle-speed number this calculator produces.
Does this formula work for drilling as well as milling?
The spindle-speed formula, n = 1000·Vc ⁄ (π·D), is identical for drilling. The feed side differs: drilling feed is usually quoted per revolution rather than per tooth, so the feed-rate step here — which multiplies by flute count — is specific to multi-flute milling cutters.
What is chip thinning and does this calculator account for it?
No. This calculator assumes the tool is engaged across a large enough radial slice that each flute cuts a chip as thick as the programmed feed per tooth. When the radial depth of cut drops below roughly half the tool diameter, the actual chip thins out, and machinists compensate by raising fz beyond the value used here — a separate adjustment layered on top of this result.
Why is there a factor of 1000 in the spindle-speed formula?
It reconciles units. Cutting speed is entered in metres per minute while the tool diameter is entered in millimetres; multiplying Vc by 1000 converts it to millimetres per minute so both quantities in the division, n = 1000·Vc ⁄ (π·D), share the same length unit before the diameter cancels out to leave a rate in revolutions per minute.