Skip to content
STEELTOETOOLS

SFM to RPM Calculator — Spindle Speed and Feed Rate

Spindle speed is not a property of the tool: it depends on the diameter turning in the machine. This calculator converts a cutting speed in surface feet per minute into RPM for the diameter you enter, works the other way round from an RPM you already have, and turns chip load and flute count into a feed rate in inches per minute.

SFM
From the tool manufacturer's catalog, for this cutter in this material. There is no speed table on this page.
in
Cutter diameter when milling or drilling; the diameter being cut on the workpiece when turning — not the largest diameter of the bar.
Number of cutting edges on the tool. A drill counts as 2.
in
Chip per tooth from the tool catalog for this diameter and material. Feed rate is meaningless without it.

Results are estimates for planning purposes. Verify with your supplier, engineer, or a qualified professional before ordering material or performing work.

Same cutting speed, four diameters

Surface speed is a property of the material and the cutting edge. Spindle speed is what the machine has to do to deliver it on the diameter that is turning, and it moves inversely with that diameter.

Spindle speed required to hold 300 SFM at four cutter diameters
DiameterCutting speedSpindle speedWhat it tells you
1/8 in end mill300 SFM9,167 RPMSmall tools run out of spindle before they run out of speed.
1/2 in end mill300 SFM2,292 RPMThe example most catalogs are written around.
1 in end mill300 SFM1,146 RPMDouble the diameter, half the RPM — every time.
3 in face mill300 SFM382 RPMA big face mill turns slowly and still cuts at the same surface speed.

The 300 SFM here is only a round number to compare against, not a recommendation. On a lathe the same rule is why a facing cut loses surface speed as the tool reaches center — constant surface speed exists to fix exactly that.

Where the two numbers you type in should come from

The arithmetic on this page is settled. The inputs are not, and they are what decides whether the tool survives the cut.

  • Cutting speed belongs to the pairing of a cutting edge and a material: substrate, coating, coolant, and whether you are roughing or finishing. The tool manufacturer publishes it for their product, usually as a range per material group. That catalog page is the source — not a generic chart, and not the number that worked on a different tool last year.
  • Chip load per tooth is published the same way, and it usually scales with the diameter and the depth of cut. Below the published range the edge rubs instead of cutting, which builds heat, work-hardens stainless and nickel alloys, and kills the tool faster than running heavy.
  • Rigidity moves both of them down. Long stickout, a thin wall, a part held in soft jaws, a worn spindle or an old knee mill will chatter at numbers that a rigid machining center eats without noticing.
  • The first cut is a test, not a commitment. Start inside the published range, listen, look at the chips, and adjust. Chip color and sound tell you more than any calculator.

The exact formula and the shop shortcut

TC 9-524 gives the exact relation, RPM = 12 × SFM ÷ (3.1416 × D), and then simplifies it for mental arithmetic to 4 × SFM ÷ D. The two are not the same: 12 ÷ π is 3.82, not 4, so the shortcut runs about 4.7 % fast. On a belt-driven drill press with six speeds that difference disappears into the next pulley step. On a machine that will hold whatever you dial in, use the exact figure — which is what this calculator returns.

The metric shortcut in the same manual, RPM = Vc × 320 ÷ D, is much closer: 1,000 ÷ π is 318.3, so it is only half a percent high.

Around the machine

  • Guards stay on. 29 CFR 1910.212(a)(1) requires methods that protect the operator from rotating parts, nip points and flying chips, and (a)(3)(ii) requires the point of operation to be guarded.
  • No gloves, no loose sleeves, no rings, no lanyards near a turning spindle. Anything that can be caught will take the hand with it.
  • Eye protection for chips, and a brush or a hook for clearing them — never a bare hand, and never while the spindle turns.
  • Do not blow chips off with shop air above 30 psi. 29 CFR 1910.242(b) limits compressed air used for cleaning to less than 30 psi, with effective chip guarding and PPE.
  • Metalworking fluid mist and skin contact are exposures in their own right; follow the safety data sheet and your employer's controls.

How it's calculated

Spindle speed from cutting speed
RPM = (12 × SFM) / (π × D)
Twelve inches of surface for every foot, divided by the circumference of the diameter turning. Shops shorten 12 / π = 3.8197 to a round 4, which gives an answer about 4.7 % high.
Cutting speed from spindle speed
SFM = (π × D × RPM) / 12
The same relation read backwards — what your surface speed really is once the machine is set to a speed it actually has.
Metric form
RPM = (1,000 × Vc) / (π × D)
With the cutting speed Vc in meters per minute and the diameter D in millimeters. TC 9-524 shortens 1,000 / π = 318.3 to 320.
Feed rate
IPM = CPT × N × RPM
Chip per tooth × number of teeth × spindle speed. In metric, mm/min = chip per tooth (mm) × teeth × RPM.
Feed per revolution
IPR = CPT × N
The distance the tool advances in one turn. On a lathe this is the number you dial in directly.

Frequently asked questions

RPM = 12 × SFM ÷ (π × diameter in inches). At 300 SFM with a 1/2 in end mill that is 3,600 ÷ 1.5708 = 2,292 RPM. The 12 turns feet into inches and the π × D is the circumference the cutting edge travels each turn.

It is 12 ÷ π = 3.8197, the whole constant of the exact formula rolled into one number, so RPM = 3.82 × SFM ÷ D. TC 9-524 rounds it further to 4 for shop arithmetic, which puts the answer about 4.7 % high — fine for setting a belt-driven drill press, not for a dialed-in CNC.

Whichever one is turning. Milling and drilling, the tool turns, so use the cutter diameter. Turning and boring, the work turns, so use the diameter being cut at that moment — which is why a facing cut has to change speed as it approaches center, and why constant surface speed exists on a lathe.

Multiply the chip load per tooth by the number of teeth and by the RPM: IPM = CPT × N × RPM. A four-flute cutter at 2,292 RPM with a 0.003 in chip load feeds at 0.003 × 4 × 2,292 = 27.5 in/min.

Because the right cutting speed belongs to the tool, the coating, the material, the coolant and the rigidity of your setup, and the numbers are published by the tool manufacturer for their product. Reproducing a general speed table here would give you a figure that looks authoritative and fits nothing. Take the SFM and the chip load off the catalog page or the box for the tool in your hand.

Take the next speed below rather than above, and put the surface speed back through this calculator in the other direction to see what you actually have. Tool life falls off quickly above the recommended speed and only slowly below it, which is why TC 9-524 tells the operator to use the slower of two speeds when conditions vary.

Chip load is what the tool cares about, so if you cut RPM to fit the machine, cut the feed rate in the same proportion and the chip per tooth stays where the manufacturer put it. Running a much lighter chip is not safe by default: too little feed rubs instead of cutting, work-hardens some alloys and burns edges.

Yes for the speed. RPM from surface speed is the same arithmetic whatever the operation. On the feed side, a drill takes two cutting edges, so IPM = chip load × 2 × RPM; on a lathe the feed is normally set per revolution rather than per minute, which is the chip load times the number of cutting edges.

Sources & references

Content checked against these sources — last reviewed September 1, 2026.

By — Editorial team of SteelToeTools.com (published by LSEA SAS) Updated v1