Cutting Speed Calculator (SFM to RPM)
Convert surface speed to spindle RPM for milling, turning and drilling, in inch or metric, with the recommended speed band for the material and tool.
How to use this calculator
- 1Pick the material and the tool material first - together they set the surface speed, which is the only part that involves judgement.
- 2Enter the diameter of whatever turns: the cutter for milling and drilling, the workpiece for turning.
- 3Use the tool maker's recommended speed when you have one. A general table cannot know about the grade, coating or edge preparation.
- 4Enter your machine's top speed so the page can tell you when the answer is unreachable rather than pretending it is not.
How the calculation works
RPM = surface speed x 12 / (pi x diameter) [inch, sfm]
RPM = 1000 x Vc / (pi x diameter) [metric, m/min and mm]
Surface speed = pi x diameter x RPM / 12- Surface speed
- How fast the cutting edge moves through the metal. A property of the material and tool pairing, not of the machine
- Diameter
- Of whatever is turning - the cutter in milling and drilling, the workpiece in turning
- The 12
- Converts feet per minute to inches per minute, so the units cancel. The metric form uses 1000 for millimetres to metres
The relation is exact. All the judgement is in choosing the surface speed, which is why the recommended band matters more than the arithmetic.
In turning, the diameter changes as the cut progresses. A constant surface speed control on a lathe raises the spindle speed as the part gets smaller for exactly this reason - facing to centre at fixed rpm means the surface speed falls to zero at the middle.
Halving the diameter doubles the required spindle speed for the same surface speed. This is the whole reason small tools are hard to run.
Worked example
A half inch coated carbide end mill in mild steel
- 1.Coated carbide in low carbon steel runs 375 to 625 sfm; the middle is 500.
- 2.RPM = 500 x 12 / (pi x 0.5) = 6000 / 1.5708 = 3820 rpm.
- 3.The band as a whole is 2865 to 4775 rpm on this diameter.
- 4.A 6000 rpm mill covers it comfortably, so nothing is capped.
Result: 3820 rpm at 500 sfm
The same cutter in high speed steel
- 1.High speed steel in the same steel runs 80 to 120 sfm - a fifth of what carbide will take.
- 2.The middle is 100 sfm, so RPM = 100 x 12 / (pi x 0.5) = 764 rpm.
- 3.Same cutter, same metal, same machine: 764 rpm instead of 3820.
- 4.That five-fold difference in spindle speed is a five-fold difference in feed rate and in cycle time, which is why carbide displaced high speed steel for production work.
Result: 764 rpm - a fifth of the carbide speed
A small cutter the machine cannot spin fast enough
- 1.Uncoated carbide in wrought aluminium runs 600 to 1500 sfm; the middle is 1050.
- 2.On a 1/8 in cutter that is 1050 x 12 / (pi x 0.125) = 32,086 rpm.
- 3.The machine stops at 6000, which is 196 sfm - about 19% of the intended surface speed.
- 4.The cut will still happen, but the feed rate has to come down in proportion, and the tool spends most of its time rubbing rather than shearing. This is the case for a high-speed spindle, not for a faster feed.
Result: 32,086 rpm wanted, 6000 available - 19% of the intended speed
Working backwards from a lathe setting
- 1.Turning 2 in diameter stainless at 1200 rpm.
- 2.Surface speed = pi x 2 x 1200 / 12 = 628 sfm.
- 3.Coated carbide in austenitic stainless wants 250 to 438 sfm.
- 4.So 628 is well above the band - the insert will not last. Around 660 rpm would put it in the middle.
Result: 628 sfm - above the 250-438 band for this pairing
Why surface speed rather than RPM
What wears a cutting edge is the distance it travels through metal and the temperature that generates. Neither has anything to do with how fast the spindle turns - a tooth on a two inch cutter at 500 rpm is moving four times as fast through the work as a tooth on a half inch cutter at the same 500 rpm, and it wears four times as fast.
So the tables that matter are written in surface speed: feet per minute in the inch world, metres per minute everywhere else. That figure belongs to the pairing of work material and tool material, and it barely moves when you change machine, holder or setup. Spindle speed is what you dial in to achieve it, and it depends entirely on diameter.
The whole conversion is one line of geometry. The edge travels pi times the diameter every revolution, so surface speed is pi x D x RPM, with a unit factor to tidy up feet or metres. Everything else on this page is about what to do when the number that comes out is inconvenient.
The small tool problem
Because spindle speed is inversely proportional to diameter, the required RPM climbs sharply as tools get small. A 1/8 inch carbide end mill in aluminium wants somewhere over 30,000 rpm to reach its proper surface speed. A 1/16 inch one wants over 60,000. Most vertical mills stop somewhere between 3,000 and 10,000.
This is the real reason small tooling is difficult, and it is not the reason most people assume. The problem is not that tiny end mills are fragile - they are, but that is manageable. The problem is that a normal machine physically cannot spin them fast enough to cut, so the edge ploughs and rubs instead of shearing. Rubbing generates heat without removing metal, work hardens the surface in stainless, and dulls the edge, which makes it rub more.
The honest options are a high-speed spindle attachment, a larger tool where the geometry allows, or accepting a long cycle time and a short tool life. What does not work is raising the feed per tooth to make up for the lost speed - that adds load to an edge that is already struggling, and small tools break in bending, not in wear.
Reading a speed band honestly
A published range is not a menu where the top end is the ambitious choice and the bottom is the safe one. Both ends have failure modes.
Running above the band shortens tool life very steeply - the relationship between speed and life is a power law, and a 20% speed increase can halve the life. That is often a perfectly reasonable trade when the machine time is worth more than the insert, which is why production shops sometimes deliberately run hot. It is a decision, not an accident.
Running below the band is the one people underestimate. Carbide is designed to work hot; below its intended speed the chip does not form cleanly, built-up edge welds workpiece material to the tool, and the edge chips rather than wearing gradually. High speed steel is far more forgiving here - it is genuinely happy running slowly - which is why it remains the right choice on a manual machine with a limited top speed.
And in every case the table is a starting point that assumes a rigid setup. A long reach tool, a light machine or a part on parallels in a vice will all want less than the book. Take the number, listen to the cut, and adjust.
What this assumes, and where it stops
Assumptions
- Surface speed bands are typical published starting values for the material and tool pairing, in good condition with adequate coolant.
- The tool is running at its nominal diameter. A worn or reground cutter is smaller than it says.
- Rigidity is adequate. Every published speed assumes it, and a marginal setup will want considerably less.
- Material hardness is near the middle of the usual range for the grade. Hardness moves surface speed more than anything else on this page.
Limitations
- It does not choose the feed. Speed and feed are separate decisions and both have to be right; a correct RPM with a wrong chip load still destroys tools.
- Coating, grade and edge preparation move the usable speed a long way, and a tool maker's recommendation for a specific tool always beats a general table.
- It says nothing about depth of cut or radial engagement, which govern the force and the power rather than the surface speed.
- Interrupted cuts, scale, castings and welded seams all call for lower speeds than solid stock of the same material.
- Very high speed machining has its own regime where the guidance here stops applying.
Common questions
What is the formula for RPM from SFM?
RPM = SFM x 12 / (pi x diameter in inches). The 12 turns feet into inches so the units cancel. Metric is the same idea: RPM = 1000 x Vc / (pi x diameter in mm). Many shops use the approximation RPM = 4 x SFM / diameter, which is about 5% high because it rounds 12/pi from 3.82 up to 4.
Is the 3.82 or the 4 version right?
12/pi is 3.8197, so that is the exact one. The shortcut of 4 x SFM / D is deliberately about 5% fast and exists because it can be done in your head at the machine. For a starting speed the difference is inside the noise; for a documented process, use the exact form.
Why does my small end mill need such a high RPM?
Because spindle speed is inversely proportional to diameter. Halving the tool doubles the RPM needed for the same surface speed. A 1/8 in carbide cutter in aluminium wants over 30,000 rpm, which most mills cannot do - so the tool ends up rubbing instead of cutting, which is why small tooling usually needs a high-speed spindle rather than just a careful hand.
What happens if I run slower than the recommended speed?
With high speed steel, very little - it tolerates running slow well. With carbide it is a real problem: carbide is designed to run hot, and below its band you get built-up edge and chipping rather than gradual wear. If your machine cannot reach carbide speeds, high speed steel is often the better tool, not the compromise it sounds like.
Does surface speed change as I turn a part down?
Yes, and this catches people out. In turning it is the workpiece diameter that counts, so at a fixed spindle speed the surface speed falls as the part gets smaller - reaching zero at the centre when facing. Constant surface speed control on a CNC lathe raises the RPM to compensate, which is why it needs a spindle speed limit set as well, or it will try to spin to infinity at centre.
Sources
- Machining Doctor - cutting speed and spindle speed — Machining Doctor
Formula and content last reviewed on .
Results are estimates for information only, not professional advice.
Related calculators
Tools people commonly use alongside the cutting speed calculator (sfm to rpm).