Cutting speed, RPM and feeds

November 3, 2026  ·  Indumor

The lathe was left at 450 rpm because the last job was a 60 mm steel shaft, and it came out fine. Now there is a 20 mm bronze bushing to make and nobody touched the levers. At 450 rpm a 20 mm diameter runs at 28 m/min (92 sfm), less than half of what bronze takes with high-speed steel: the part comes out the same, only two or three times slower, and since "it always ran like that" nobody notices. The opposite mistake costs more. A 200 mm stainless part at those same 450 rpm runs at 283 m/min and burns the HSS edge on the first pass.

The rpm formula

What the cutting edge sees is how fast the material goes past it, measured at the periphery of the workpiece (or of the tool, when the tool is what turns). That is the cutting speed, Vc, in meters per minute. Each revolution the periphery travels π·D millimeters; in n revolutions, π·D·n; divided by 1000, meters.

For mental arithmetic, n ≈ 320·Vc/D, since 1000/π is 318. At 25 m/min on a 40 mm bar, 320 × 25 / 40 gives 200 rpm. A geared head never has the exact number, so take the nearest speed below, or above if the gap is small and the tool is carbide. American catalogs give the speed in surface feet per minute (sfm); divide by 3.28 for m/min, or use n ≈ 4·sfm/D with D in inches, which is the same sum (the factors are in chapter 1).

Cutting speeds by material

No speed chart is exact, this one included. What an edge will stand depends on the real hardness of the material, on the tool, on the rigidity of the machine and the setup, on coolant, and on the tool life you are willing to accept: catalog values usually aim at roughly 15 minutes of continuous cutting between regrinds or insert changes in turning, and about 45 in milling and drilling (tool-life tests for lathe tools follow ISO 3685). On a lathe with play and a long part between centers, start at the low end of the range.

Reference hardness: 1010-1020 about 120 HB, 1045 about 200 HB, 4140 Q&T 28 to 32 HRC, annealed tool steel about 220 HB. Multiply by 3.28 for sfm. On the saw, figures up to 120 m/min are for a horizontal machine; aluminum and plastics take far more on a fast vertical saw (aluminum, 2000 m/min or more).

For carbide the chart is only a starting point, because every insert grade has its own range. What is universal is the ISO 513 classification, six letters with a color each (the blue box is for steel, the yellow for stainless, the red for cast iron) and a number that gives the application. P10 is a hard grade for high-speed finishing, P40 a tough one for roughing and interrupted cuts.

RPM chart by diameter

With the speed chosen, the chart gives the rpm without the arithmetic. For milling cutters and drills D is the tool diameter; on the lathe it is the workpiece, and when facing or parting it changes along the pass, and at the center the cutting speed is zero. A printed copy of this chart hangs beside every machine in our shop.

Feeds: per revolution and per tooth

Cutting speed says how fast the material goes past the edge; feed says how far the edge advances each revolution. On the lathe and the drill press it is measured in millimeters per revolution (f). On the mill, the figure that belongs to the tool is the feed per tooth, fz, also called chip load: how far the part advances between one tooth and the next. A four-flute cutter at 0.1 mm per tooth advances 0.4 mm per revolution, and the table feed rate, Vf, is that feed times the rpm, which is the number you dial into the milling machine, in mm/min (inches per minute, ipm, on an inch machine).

In finishing, the lathe feed is limited by the nose radius of the tool; f should not exceed half that radius, or the feed marks show (the roughness each feed leaves is in chapter 14). Roughing is limited by power and rigidity. In drilling the feed grows with the diameter, one or two hundredths of a millimeter per millimeter of drill in steel; the drill itself is in chapter 10.

There are two ways a milling cutter can attack the material. In conventional (up) milling the part feeds against the rotation: the chip starts thin and ends thick, the tooth rubs before it bites and the cutter tends to lift the part. In climb (down) milling the part feeds with the rotation: the chip starts thick and ends thin, the tooth bites at once and the cutter pushes the part down onto the table, with a better finish and less wear. But it needs a table with no backlash in the lead screw, because the cutter pulls the part forward at every tooth; old machines are run in conventional milling unless they have a backlash eliminator.

Cutting time and power

From the feed rate comes the time for the pass, the length divided by Vf, adding the tool's entry and exit (for a face mill, its diameter; for a drill, the height of the point). It is useful for quoting and for comparing: if the sum says two minutes and the pass takes eight, something is wrong with the rpm or the feed.

The cutting power comes from the volume of chips per minute multiplied by the specific cutting force kc, the force it takes to remove one square millimeter of chip cross-section. kc rises when the chip is thin, because the edge then deforms more than it cuts; the Kienzle formula expresses it with a base value kc1 for a chip 1 mm thick and an exponent mc.

These are the classic Kienzle values; they agree with the kc curves published by insert makers for carbon and chromium-molybdenum steels and for gray iron. Other tables give quite a bit less: for C45, a base value of 1450 to 1500 N/mm² with mc of 0.22 to 0.27, and for 4140, 1565 to 1775. Use them to estimate power, on the safe side, and no further. The figure for plastics is only an order of magnitude.

The motor has to deliver more than the cut takes, because the drive loses some; with belts and a gearbox, count on an efficiency of 0.7 to 0.85. When the sum comes out above what you have, reduce the depth of cut before the speed, since that is what lengthens the total time the least (power, torque and speed: chapter 24).

Calculator

Frequently asked questions

How do you calculate lathe rpm?

With n = 1000 · Vc / (π · D): the cutting speed in m/min times 1000, divided by π and by the workpiece diameter in mm. For a 50 mm shaft at 30 m/min, 1000 × 30 / (3.14 × 50) = 191 rpm. In inch units, n ≈ 4 · sfm / D with D in inches.

What cutting speed is used for steel with high-speed steel tools?

Between 20 and 40 m/min (65 to 130 sfm) for ordinary carbon steels, 12 to 20 m/min for quenched-and-tempered alloy steels and stainless. With coated carbide inserts multiply by five or more. They are guide ranges: real hardness, machine rigidity and coolant move them.

What is the difference between feed per revolution and feed per tooth?

Feed per revolution (f, mm/rev) is how far the tool advances in one turn of the workpiece or the drill. Feed per tooth (fz, chip load) is how far the part advances between two consecutive teeth of a milling cutter; times the number of teeth it gives the feed per revolution, and times the rpm, the table feed rate in mm/min.

Sources: ISO 3685:1993 (tool-life testing with single-point turning tools); ISO 513:2012 (classification of hard cutting materials); DIN 6580 (kinematics and geometry of the cutting process); DIN 6584 (cutting forces, energy and power); O. Kienzle, Die Bestimmung von Kräften und Leistungen an spanenden Werkzeugen (1952); Machinery's Handbook, 31st edition (2020), Speeds and Feeds; tool manufacturers' catalogs.