Feeds & Speeds Calculator
Spindle speed, feed rate, chip load and material removal rate for milling and turning — worked in whichever direction you need. It also checks the answer against a real machine list, because an RPM your spindle can't reach isn't an answer. Every result shows its formula.
Or set RPM below and this back-calculates.
Type here to work backwards to Vc.
Type here to work backwards to Vc.
Feeds and speeds — the arithmetic, and what it can't tell you
The arithmetic is genuinely simple, and it is worth knowing rather than trusting a black box. Spindle speed comes from cutting speed and diameter: RPM = (Vc × 1000) ÷ (π × D). Feed rate comes from spindle speed, the number of teeth and the feed per tooth: Vf = RPM × z × fz. Material removal rate for milling is MRR = (ap × ae × Vf) ÷ 1000 cm³/min. That is the whole of it — every feeds and speeds calculator on the internet is doing those three lines.
What that arithmetic cannot tell you is what Vc and fz should be, and that is the part that actually matters. Those depend on the specific insert grade, its coating, the edge geometry, how rigid your setup is, whether you have through-tool coolant, and how much overhang the tool has. A generic "aluminium = 300 m/min" band is a starting point, not an instruction. This is why we publish the bands as broad ranges and tell you plainly to use your tooling supplier's data — they tested their own inserts; nobody else did.
Two things the formulas hide. First, chip thinning: when radial engagement (ae) drops below half the cutter diameter, the actual chip is thinner than your programmed fz, so you can — and generally should — feed faster to keep the chip at a sensible thickness. Feed too lightly at low radial engagement and you rub rather than cut, which destroys tools faster than being aggressive does. Second, rigidity beats theory: a perfect calculation through a long, thin tool in a marginal fixture will chatter regardless of what the numbers say.
The check this calculator adds that a generic one cannot: it compares the required RPM against a real machine list — our own fleet, from a 12,000 RPM DN Solutions DVF 5000 5-axis down to a 3,500 RPM Doosan Puma GT 2600. Small cutters in aluminium routinely ask for spindle speeds a heavy turning centre simply cannot deliver, and the honest answer is then "use a different machine or accept a lower Vc" rather than a number you can never program.
Feeds and speeds — FAQ
How do you calculate RPM from cutting speed?
RPM = (Vc x 1000) / (pi x D), where Vc is cutting speed in m/min and D is the cutter or workpiece diameter in mm. For example, 120 m/min with a 10 mm cutter gives (120 x 1000) / (3.1416 x 10) = 3,820 RPM.
How do you calculate feed rate for milling?
Feed rate Vf = RPM x number of teeth x feed per tooth. A 4-flute cutter at 3,820 RPM with 0.05 mm/tooth gives 3,820 x 4 x 0.05 = 764 mm/min.
What is chip load?
Chip load is the feed per tooth (fz) — the thickness of material each cutting edge removes per revolution. It is the number that actually protects your tool: too high overloads the edge, too low causes rubbing instead of cutting, which work-hardens the surface and kills the tool faster than being aggressive.
What is chip thinning?
When radial engagement is less than half the cutter diameter, the actual chip is thinner than the programmed feed per tooth. To keep the real chip thickness sensible you need to increase the feed. Failing to compensate is a common cause of poor tool life in light radial passes.
What cutting speed should I use for aluminium, stainless or titanium?
It depends entirely on your tooling, not just the material. As broad starting bands: aluminium is fast, stainless is moderate, and titanium and nickel superalloys are slow with conservative parameters. Always use your insert manufacturer published data for their specific grade and coating — it beats any generic chart.
How do you calculate material removal rate?
For milling, MRR = (axial depth x radial width x feed rate) / 1000, giving cm3/min. It is a useful way to compare two strategies — a light, fast pass versus a deep, slow one — on a like-for-like basis.
Send Your Drawing for a Same-Day Quote
Talk directly to the engineers who will machine your parts — no account managers, no trading-company markups. Complimentary DFM review with every enquiry.