SFM to RPM conversion

SFM — surface feet per minute — is the speed at which the cutting edge of a tool passes through the material, measured at the cutting diameter. It is the number machinists actually care about, because it is a property of the material and tool, not of the machine. A spindle, by contrast, is set in RPM (revolutions per minute). Converting between the two is the single most common piece of arithmetic on the shop floor: you look up the right cutting speed for the job, then translate it into a spindle speed for the diameter you are running.

The imperial formula

Spindle RPM is the surface speed divided by the circumference of the cut. With the diameter D in inches and SFM in feet per minute:

RPM = (SFM × 12) / (π × D)

The 12 converts feet to inches so the units agree. Because 12/π ≈ 3.82, this is almost always written in the shorthand machinists keep in their heads:

RPM = 3.82 × SFM / D

D is the cutting diameter — the tool diameter for a drill or end mill, or the workpiece diameter for turning. Note the inverse relationship: halving the diameter doubles the RPM for the same surface speed, which is why small drills and engravers spin so fast.

The metric formula

In metric the cutting speed is called Vc and is given in metres per minute (m/min), with the diameter D in millimetres:

n = (1000 × Vc) / (π × D)

Here the 1000 converts metres to millimetres so the units cancel. The structure is identical to the imperial version — surface speed over circumference — only the unit-conversion constant changes.

Converting RPM back to SFM

To go the other way — for example, to check whether a spindle speed you have set lands in the recommended range — just rearrange:

SFM = π × D × RPM / 12  (D in inches)

Vc = π × D × n / 1000  (D in mm)

This is handy when a machine has a fixed set of gear speeds: pick the nearest available RPM, then back-calculate the actual surface speed to confirm you are still in a sensible window for the material.

What SFM should you use?

The cutting speed depends on the workpiece material and the tool material, and to a lesser extent on coolant, rigidity and depth of cut. These are starting points, not hard limits — treat them as the centre of a range and tune for tool life and finish:

• Mild steel: roughly 80–120 SFM with HSS tooling, climbing to about 300–600 SFM with carbide.
• Aluminium: much higher — often several hundred SFM with HSS and well into four figures with carbide, because it cuts so freely.
• Tool steel and other hard alloys: lower than mild steel, since the heat and abrasion at the edge climb quickly.

For a fuller breakdown by material and tool type, see the cutting speed chart. Once you have a feed rate to pair with the RPM, the CNC speeds and feeds calculator rolls spindle speed, feed and material removal rate into one calculation.

Why surface speed matters more than RPM

It is tempting to think of a job in terms of spindle speed, but the cutting edge does not feel RPM — it feels surface speed. A tool turning at a fixed RPM cuts faster at a large diameter and slower at a small one, because the edge travels a longer path per revolution on a bigger circle. That is why a single recommended SFM, converted to the right RPM for each diameter, keeps the edge in its happy zone across a whole range of tools and parts.

Run too far above the recommended SFM and the heat at the edge climbs sharply: the tool dulls, work-hardens the surface, and can fail outright. Run too far below it and you waste cycle time, risk rubbing instead of cutting, and on some materials promote built-up edge that ruins the finish. The convert-to-RPM step exists so you can dial in that surface speed precisely for the diameter in front of you.

A quick sanity check by eye

Because 12/π ≈ 3.82, a useful rule of thumb is that for a 1-inch diameter the RPM is just the SFM times 3.82 — so 100 SFM is about 382 RPM at 1 inch. Halve the diameter and the RPM doubles; double it and the RPM halves. With that single anchor you can ballpark almost any speed in your head before reaching for the calculator, then let the tool confirm the exact figure.

Worked example — imperial

You are running a 1/2" (0.5 in) HSS end mill in mild steel and pick a cutting speed of 100 SFM:

RPM = 3.82 × 100 / 0.5 = 764 RPM

So you would set the spindle to about 764 RPM. If your machine only offers 700 or 800 RPM, either is close enough — back-calculate to confirm: at 800 RPM the surface speed is π × 0.5 × 800 / 12 ≈ 105 SFM, still well inside the HSS range for steel.

Worked example — metric

The same job in metric units: a 12 mm cutter at a cutting speed Vc = 30 m/min:

n = 1000 × 30 / (π × 12) = 30 000 / 37.7 ≈ 796 rpm

That lands you at roughly 796 rpm — the same neighbourhood as the imperial example, as you would expect for comparable cutting conditions. (Both of these are exactly what the calculator returns for these inputs.)

Common mistakes

The two errors that bite most often are using diameter in the wrong units — feeding millimetres into the imperial formula or inches into the metric one — and using the nominal tool size instead of the true cutting diameter. For a ball-nose cutter at a shallow depth, or a turning pass on a tapered part, the effective diameter at the cut can be well below the nominal size, which raises the correct RPM. When in doubt, compute from the diameter that is actually engaged in the material.

Frequently asked questions

What is the SFM to RPM formula?

In inches, RPM = (SFM × 12) / (π × D), which simplifies to RPM = 3.82 × SFM / D, where D is the cutting diameter in inches. In metric, n = (1000 × Vc) / (π × D), with Vc in m/min and D in mm.

Is SFM a property of the machine or the material?

SFM (surface feet per minute) is the cutting speed at the tool’s cutting edge, and it is set by the workpiece material and tool material — not by the machine. You look the SFM up first, then convert it to a spindle RPM for the diameter you are running.

How do I convert RPM back to SFM?

Reverse the formula: SFM = π × D × RPM / 12 with D in inches, or Vc = π × D × n / 1000 with D in mm. This is useful for checking whether a known spindle speed lands you in the recommended cutting-speed range for the material.

Last reviewed: 2026-05-29.