The catalog gives you a cutting speed, the machine wants RPM and a feed rate. This calculator does the conversion both ways, metric or inch, for turning, milling and drilling, and offers carbide starting values by ISO material group when you have nothing else to go on. Runs entirely in your browser, nothing is sent anywhere.
Starting values are turning ranges for coated carbide unless noted; milling and drilling verified values come from your tool maker's data. This calculator does the unit math; it does not know your setup's rigidity, coolant or tool condition.
For a drill, Vc applies at the outer diameter; at the centre of the drill the cutting speed is zero. That is one reason drilling data for the same material sits below turning data, and why the maker's drilling feed per revolution is the number to trust, not a turning feed carried over.
Same table as our speeds & feeds guide: starting ranges from common practice for coated carbide turning, not gospel and not from any one catalog. Start mid-range, then let the chip and the wear move you.
| Group | Starting Vc (m/min · sfm) | Feed fn (mm/rev · ipr) | Notes |
|---|---|---|---|
| P Steel | 150–350 · 490–1150 | 0.1–0.5 · .004–.020 | Lower for hard alloy steel and roughing, higher for finishing with a coated grade |
| M Stainless | 120–220 · 395–720 | 0.15–0.4 · .006–.016 | Austenitic work-hardens; keep the tool moving, sharp positive geometry, flood |
| K Cast iron | 100–250 · 330–820 | 0.2–0.5 · .008–.020 | Grey iron higher than ductile; usually dry |
| N Aluminium | 300–1200+ · 985–3940+ | 0.05–0.3 · .002–.012 | Sharp polished high-rake tools; very high speed is fine, keep chips clearing |
| S Titanium | 30–70 · 100–230 | 0.1–0.25 · .004–.010 | Heat-limited; copious coolant, rigid setup, do not let it dwell |
| S Nickel superalloy | 15–50 · 50–165 | 0.1–0.25 · .004–.010 | Inconel and similar; very heat-limited, rigidity is everything |
| H Hardened steel | 100–250 (CBN/ceramic) · 330–820 | 0.05–0.2 · .002–.008 | Hard turning with CBN or ceramic; carbide runs far slower here |
Subgroup, grade, coating, operation, coolant and rigidity all shift the number. For the grounded per-insert value, ask the advisor.
Multiply the cutting speed by 1000 and divide by π times the diameter: n = (1000 × Vc) / (π × D), with Vc in m/min and D in mm. Example: Vc 200 m/min on a 50 mm diameter is (1000 × 200) / (3.1416 × 50), about 1273 rpm. In inch units, n = (12 × SFM) / (π × D in inches).
Feed per revolution (fn, mm/rev) is how far the tool advances in one spindle revolution; it is the feed unit for turning and drilling. Feed per tooth (fz, mm) is how much material each cutting edge of a milling cutter removes per engagement. A milling feed rate is n × fz × z, so the same fz gives a very different table feed on a 2-flute and a 10-flute cutter.
Run at the machine's maximum and accept the lower effective cutting speed; this is routine on small diameters, where the RPM for a normal Vc becomes enormous. Note the actual Vc you end up with (this calculator's back-check row shows it), because tool life expectations from the catalog assume the catalog's Vc, not yours.
1 m/min is about 3.28 sfm, so divide SFM by 3.28 to get m/min, or multiply m/min by 3.28 to get SFM. The inch toggle on this calculator does this for you and also switches the diameter to inches and the feed units to ipr/ipm.
They are the coated-carbide turning starting ranges published in our speeds & feeds guide, compiled from common practice, deliberately wide, and not from any one catalog. Do not use them when you have the insert maker's data for your exact grade and operation; the verified number always wins. For a grounded per-insert recommendation, ask the advisor.
This page converts numbers you already have. The advisor is for the number you do not have: which grade, geometry and cutting data for your material and operation, grounded in catalog data across 13 brands, brand-neutral.