Cutting Speed Calculator — SFM and m/min by Material and Tool

Cutting speed (vc) is how fast the tool edge travels across the material, in metres per minute or surface feet per minute. Spindle speed (n) is how fast the machine turns, in rpm. They are linked by diameter: vc = pi x D x n / 1000 for metric, so the same recommended cutting speed produces a different rpm on every diameter. A 10 mm drill and an 80 mm face mill asking for the same 100 m/min run at about 3183 rpm and about 398 rpm respectively — this is why a chip-load chart alone will not set a machine.

Metric: rpm = (cutting speed in m/min x 1000) / (pi x tool diameter in mm), which is the same as cutting speed x 318 / diameter. Inch: rpm = (surface speed in SFM x 3.82) / tool diameter in inches. Both are worked through with real numbers in the steps below, and the ISO and vendor rows above give the cutting speed to feed into them.

Start in the lower half, prove tool life and surface finish on a few parts, then move up. The upper figure in a vendor range assumes a rigid setup, a first-choice grade, flood coolant and stable workpiece support; a job on an older machine, a long overhang or an interrupted cut lives in the lower half. If you are between two grades, take the speed that suits the weaker of the two, not the average.

Match it to the ISO group first: P for steel, M for stainless, K for cast iron, N for non-ferrous, S for heat-resistant alloys, H for hardened steel. Each group above lists what belongs in it. Within a group the deciding factors are hardness and condition — annealed versus quenched and tempered changes the answer far more than the alloy name does — so send the grade and the hardness reading and we will point you at the right row rather than the nearest row.

Because those materials do not conduct heat away from the edge. In 304 stainless most of the heat generated in the cut goes into the tool rather than the chip, and titanium alloys are worse and also work-harden under the edge. Cutting them at carbon-steel speeds destroys the insert in minutes. The same mechanism is why feeds are kept up in stainless — a light rubbing pass work-hardens the surface and makes the next pass harder than the first.

Yes, the speeds are material and tool properties and do not know what units the machine uses. Convert the diameter and use the matching formula: a 0.5 in drill in mild steel at 25 m/min runs at about 627 rpm, exactly as a 12.7 mm drill would. The two tables in the rows above give both m/min and SFM so either shop can work straight from the row without converting first.

Deep holes reduce the speed and increase the trouble with chip evacuation, so start at the lower end of the vendor range and plan pecking or through-coolant. Interrupted cuts and hard scale want a tougher grade and roughly 20-30% off the recommended speed to protect the edge from the impact rather than the heat. Both cases are about the same thing: keeping the edge from reaching its thermal limit on the part of the cycle where it is weakest.

Use them to find the window, then let the machine and the tool life decide the final numbers. Vendor data is published for a reference workpiece condition and a first-choice grade, and real castings, forgings and heat lots move within a band. The practical method is to pick the row, start low, measure tool life and surface finish over a few parts, then step the speed up until either the finish or the life turns — that final setting belongs to your machine, not to a table.