SizingKitFree surface footage calculator
Surface footage is a velocity, not a spindle speed
Surface footage is how fast the cutting edge travels through the metal — feet per minute at the circumference — and a spindle speed is only that velocity divided by a diameter. This converts between the two in either direction, reports the result in SFM and m/min at once, corrects for a ball nose that is only touching the work near its tip, and prints a chart of starting bands for seven materials as rev/min for the exact tool you are holding. Free, no account, and the whole table is compiled into the page.
- 100% free
- No signup
- SFM and m/min
- Ball nose corrected
- Printable speed chart
The cutter on a mill or a drill; the workpiece on a lathe. Whatever is going round.
Vc in a European catalog is this same quantity in m/min.
CUTTING SPEED
400 SFM
121.9 m/min
SPINDLE SPEED
3,056
rev/min
- Diameter at the cut
- 0.5000 in / 12.70 mm
- Edge travel per revolution
- 1.571 in
The diameter is doing all the work here. Surface speed is how fast the edge travels through the metal, so a revolution of a 0.500 in circle carries the edge 1.571 in and nothing about the machine changes that. RPM = SFM × 12 ÷ (π × D) is that statement rearranged, with 12 ÷ π = 3.8197. Twelve inches to the foot divided by π. RPM = SFM × 12 ÷ (π × D in inches) is the definition of surface speed rearranged; the familiar 3.82 is this constant rounded, and the familiar 4 is it rounded badly, running about 5% fast.
Starting speeds by material, and the rev/min they mean at 0.5000 in
Bands in SFM with the exact metric equivalent in brackets, then what each band asks of the spindle at 0.5000 in (12.70 mm). Print this and it is a speed list for the tool in the holder rather than a generic chart.
| Material | HSS · SFM (m/min) | HSS rev/min | Carbide · SFM (m/min) | Carbide rev/min |
|---|---|---|---|---|
| Mild / low-carbon steel | 80–110 (24.4–33.5) | 611–840 | 300–600 (91.4–182.9) | 2,292–4,584 |
| Alloy steel, annealed | 50–80 (15.2–24.4) | 382–611 | 200–400 (61–121.9) | 1,528–3,056 |
| Stainless steel, austenitic | 40–70 (12.2–21.3) | 306–535 | 150–350 (45.7–106.7) | 1,146–2,674 |
| Gray cast iron | 60–90 (18.3–27.4) | 458–688 | 250–500 (76.2–152.4) | 1,910–3,820 |
| Aluminum | 250–450 (76.2–137.2) | 1,910–3,438 | 600–1500 (182.9–457.2) | 4,584–11,459 |
| Brass, free-machining | 150–300 (45.7–91.4) | 1,146–2,292 | 400–900 (121.9–274.3) | 3,056–6,875 |
| Titanium alloy | 30–50 (9.1–15.2) | 229–382 | 100–250 (30.5–76.2) | 764–1,910 |
Conventional starting surface speeds of the kind published in the Speeds and Feeds section of Machinery's Handbook and in tooling manufacturers' technical catalogs, given as a range per material class and tool material. Meters per minute are the exact conversion of the imperial figures at 0.3048 m to the foot. Unit horsepower is the power constant used for spindle power estimation in the same references.
How to convert surface speed to a spindle setting
One relation, two directions, and the one geometry that changes which diameter goes into it.
Choose which of the two you already have
Going from a catalog speed to a machine setting is the usual direction, and going back the other way answers a different and equally common question: the spindle is at 1,200 and you want to know whether that is a sensible cut. Both use the same relation, so the panel simply moves which box is an input. Nothing else changes.
Enter the diameter of whatever is going round
On a mill or a drill that is the tool, because the tool is what spins. On a lathe it is the bar, and it is falling as the cut goes on, which is why lathe controls have a constant-surface-speed mode at all. Fractions, decimals, inches and millimeters all read the same, so 1/2, 0.5 and 12.7 mm are one diameter written three ways.
Tick the ball nose box if the cutter is round and the pass is shallow
A ball nose taking less than its own radius in axial depth is not touching the work at its nominal diameter, and the width it is actually touching over is what the surface speed is measured on. A 1/2 in ball at 0.030 in depth engages over 0.2375 in, so the nominal figure asks the spindle for less than half the speed the cut needs. The panel prints both numbers side by side so the size of that mistake is visible.
Technical specifications
| Solved both directions | RPM = SFM × 12 ÷ (π × D) and SFM = π × D × RPM ÷ 12 — the same identity, one field moving between input and output |
|---|---|
| The constant | 12 ÷ π = 3.8197 exactly. The shop's 3.82 rounds it harmlessly; the shop's 4 runs 4.7% fast |
| Metric | 0.3048 m to the foot by definition, so 100 SFM is 30.48 m/min and a Vc figure from an ISO catalog can be typed in directly |
| Ball nose correction | Deff = 2√(R² − (R − ap)²) — a 1/2 in ball at 0.030 in axial depth cuts at 0.2375 in, and the nominal diameter understates the speed 2.11 times |
| Chart output | Every tabulated band converted to a rev/min range at the diameter you entered, so the printed sheet belongs to the tool in the holder rather than to the material in general |
| Input ranges | Diameter 0.01 to 24 in, cutting speed 0.5 to 20,000 in either unit, spindle speed 1 to 200,000 rev/min |
| Print behavior | The chart prints with the diameter named in its subtitle; the entry panel and the answer plate are marked screen-only and drop out |
| Offline | The band table is compiled into the page rather than fetched, so the chart is there with the network off and no figure you type leaves the tab |
Frequently asked questions
What does surface feet per minute actually measure?
The speed of the cutting edge through the metal, in feet traveled per minute — a velocity, not a rotation. Wrap a string round the circle that is turning, spin it for one minute, and SFM is how much string went past the cutting point. That is why the same 1,000 rev/min is a completely different cut on a 1/8 in cutter and a 2 in one: the small one carries its edge 3.3 feet per minute for every hundred rev/min, the big one 52. Everything about tool life is governed by that velocity and the heat it generates, and almost nothing by the shaft speed on its own.
Why does a 1/4 in cutter need a different spindle speed from a 1 in cutter in the same material?
Because the material dictates the edge velocity and the diameter decides how many revolutions produce it. At 400 SFM a 1/4 in cutter needs 6,112 rev/min and a 1 in cutter needs 1,528 — a four to one ratio, exactly the ratio of the diameters, because rev/min is inversely proportional to diameter at a fixed surface speed. The practical consequence in a shop is that the small tools are the ones your spindle cannot keep up with. A machine that tops out at 6,000 rev/min is already short of the mark for a 1/4 in carbide cutter in aluminum and hopeless for a 1/16 in one.
My insert catalog gives Vc in m/min. What do I type?
Type the m/min figure and switch the unit selector next to it — the panel converts at 0.3048 meters to the foot, which is exact by definition rather than rounded. In round terms 100 SFM is 30.5 m/min and 100 m/min is 328 SFM, so a European recommendation of 200 m/min is 656 SFM. The two are the same physical quantity under two names, and the letter Vc is simply how ISO tool documentation writes it. There is no separate conversion to learn and no fudge factor between them.
Does a ball nose cutter run at its nominal diameter?
Only when the axial depth of cut reaches its radius. Below that the ball is engaged over a narrow band near its tip, and the effective diameter is 2√(R² − (R − ap)²) — for a 1/2 in ball at 0.030 in depth, 0.2375 in rather than 0.500. Using the nominal figure understates the required spindle speed by 2.11 times, which is not a rounding error: it puts the cut at less than half the intended surface speed, where the edge burnishes rather than shears and the finish gets worse the more carefully you go. This is the single most common speed mistake in three-dimensional finishing work, and it is invisible because the tool does not break, it just wears out early and leaves a poor surface.
Where does 3.82 come from, and is 4 close enough?
It is twelve divided by π, or 3.8197 to four places — twelve inches to the foot on top, and the π that turns a diameter into a circumference underneath. Rounding it to 3.82 costs nothing measurable. Rounding it to 4, which plenty of shop charts do for mental arithmetic, runs the spindle 4.7% fast, and whether that matters depends on where you were in the band: at the top of a carbide band in stainless it is a real bite out of tool life, while at the bottom of an aluminum band nobody will ever detect it. The panel uses the exact value and prints it, so you can see which of the two you are comparing against.
Does the surface speed change when I take a deeper cut?
Not for a square end mill, which cuts on its periphery at full diameter regardless of depth, and dramatically for anything with a curved cutting edge. A ball nose changes with every change in axial depth. A drill is the extreme case: the periphery of the drill runs at the tabulated speed while the very center of the web is turning at zero surface feet per minute, which is why the chisel edge extrudes metal rather than cutting it and why split points exist at all. On a lathe the diameter falls as the cut progresses, so the surface speed falls with it unless the control is holding it constant.
Is SFM the same thing as the feed rate in inches per minute?
No, and the units are the clue: SFM is feet per minute at the edge of a spinning tool, feed rate is inches per minute of table or carriage travel. A 1/2 in four-flute cutter at 400 SFM is turning 3,056 rev/min and feeding around 37 in/min, and neither figure can be read off the other without the chip load and the flute count in between. Surface speed is set by the material and decides how hot the edge gets; feed rate is set by the chip you want each tooth to take and decides how hard the tool is loaded and how quickly the job finishes. Confusing them is common enough that a 400 typed into a feed box is a recognizable way to break a cutter.
About cutting speed, and why the machine's dial is the wrong unit for it
Cutting speed is a property of the pair of materials meeting at the edge. Carbide in gray iron will take 250 to 500 feet of iron passing under it every minute; the same carbide in Ti-6Al-4V is tabulated at 100 to 250, and the top of that band is optimistic, because titanium conducts heat so poorly that nearly all of it stays in the tool rather than leaving in the chip. Neither of those numbers has anything to do with a machine. What a machine offers is revolutions, and the diameter is the exchange rate between the two — which is why a shop's speed chart is written in SFM and a shop's spindle is set in rev/min, and why the arithmetic between them has to happen every time the tool changes. The relation itself is trivial and permanent: twelve inches to the foot, π to turn a diameter into a circumference, and no material constant anywhere in it. Everything difficult about speeds and feeds is in the SFM you choose, not in the conversion.
The failure this page is built around is using a diameter the tool is not actually cutting at. It happens constantly with ball nose cutters in three-dimensional work, where a finishing pass takes a few thousandths of axial depth and the ball is engaged over a fraction of its width; the effective diameter formula above is the correction, and the error runs the tool slow rather than fast, which is why nobody notices it until the tools start wearing out early. The same principle explains the chisel edge of a drill, which is at zero surface speed however fast the spindle turns, and it is the whole reason for constant surface speed control on a lathe. It also explains something people find surprising about gearing: a spindle speed measured at the motor is not the speed at the tool unless the drive ratio is one, and working the ratio out is a separate step on any belt or back-geared head.
The bands charted here are starting ranges for a material class, and the sensible way to read them is as a place to begin rather than a target. Hardness moves them more than alloy designation does — a 4140 bar at 180 HB and the same bar quenched and tempered to 350 HB are two different cutting problems under one part number, so a hardness conversion is often the honest first step before any of this. Once a speed is chosen, the second half of the setup is the chip, which is a different quantity with its own table and its own failure modes: the chip load page takes it from there, and the full setup panel does both at once for milling, drilling and turning.
What the chart knows about you
Every number on this page is worked out by JavaScript running in the tab you are reading it in. Nothing you type — loads, lengths, nameplate ratings, the rates your utility charges you — is uploaded, logged or kept, which is also why the calculators carry on working in a mechanical room with no signal.
The diameter you type is used to fill the last two columns of the chart and then forgotten when the tab closes. Nothing is stored, so a chart printed for a 3/8 in cutter has to be printed again for the next tool — which is the point of it being generated rather than a fixed image.