Turning (lathe) RPM calculator
On a lathe the workpiece spins, so the spindle speed follows from the workpiece diameter — enter it with the material and feed per revolution for speed and feed rate.
Turning: why the number keeps moving while you cut
Turning is the one operation where the diameter that sets your speed changes continuously during the cut. On a mill the cutter diameter is fixed all day; on a lathe it is the workpiece that spins, so every pass that takes material off makes the diameter smaller — and a smaller diameter at the same rpm means a lower cutting speed at the tool tip. Start a roughing pass at the correct speed on a 60 mm bar and by the time you are down to 40 mm the edge is running a third slower than intended, which is why the finish often deteriorates toward the end of a long cut on manual machines.
Constant surface speed, and the trap at the centre
CNC lathes solve this with constant surface speed, G96 on most controls: you program the cutting speed you want and the machine keeps adjusting rpm as the diameter changes. It works beautifully until you face toward the centre, because as the diameter approaches zero the required rpm approaches infinity. That is what the rpm clamp is for — every control has one, and setting it is not optional. Forget it and the spindle will wind up to its maximum as the tool reaches the middle, with a part that may not be balanced for that speed. On a manual lathe there is no G96 at all, so pick your speed for the diameter you will spend most of the cut at, and adjust by ear as it drops.
Feed per revolution, not per tooth
Milling feeds per tooth because several teeth pass through the cut. Turning has one edge, so feed is expressed per revolution: Vf = f × n, where f is millimetres of tool travel for each full turn of the workpiece. That single number does more for your surface finish than anything else you can change. A common roughing feed sits around 0.2 to 0.4 mm per revolution and a finishing feed of 0.05 to 0.15, but the real constraint is the tool nose radius, which is the subject below.
Nose radius: the finish comes from geometry, not from going slower
The most useful relationship in turning is that surface roughness rises with the square of the feed and falls with the nose radius of the insert. Halve your feed and the finish improves roughly fourfold; move to a larger nose radius and it improves without costing you any time at all. This is why a rough finish is so rarely fixed by reducing rpm — people try that first because it feels cautious, but rpm is not what leaves the marks. The practical rule is to keep the feed below roughly half the nose radius for a finishing pass. A larger radius does push cutting forces sideways into the workpiece, so on a long slender part it can cause chatter or push the part away from the tool, which is where you trade back.
Rigidity: overhang is the enemy on a lathe too
A workpiece sticking far out of the chuck behaves like a diving board, and the deflection grows with the cube of the length. Doubling the overhang makes the part roughly eight times more flexible, which is why a slender shaft turns beautifully near the chuck and starts to chatter and taper further out. Support anything long with a centre or a steady rest rather than reducing your numbers, because a flexible setup does not become rigid by cutting slowly. The same applies to the tool: a boring bar reaching deep into a hole is the most flexible thing in the machine, and there the usual answer is a shorter bar or a larger one, not a lighter cut.
Parting off, the operation that punishes guessing
Parting is where the numbers matter most and forgiveness is least. The tool is narrow, buried on both sides, has nowhere to send its chip, and is cutting toward a diameter that keeps shrinking — every failure mode of turning at once. Run a constant surface speed and it will accelerate to the rpm limit as the part separates. Feed too lightly and the tool rubs and work-hardens the material ahead of it, which is the usual reason a parting blade suddenly grabs and breaks. The values here are starting points for a normal outside diameter cut; when parting off, keep the tool short, keep it exactly on centre height, feed positively rather than timidly, and slow the spindle as you approach the middle.
Why the workpiece diameter sets the speed
Cutting speed is how fast material passes the tool tip. On a lathe that's the workpiece surface, so n = (Vc × 1000) / (π × Øworkpiece). It also means the correct rpm changes as you cut: turn a 40 mm bar down to 20 mm and the right speed doubles. CNC lathes automate this as constant surface speed (G96); on a manual lathe you step the speed up as the diameter shrinks.
Which tooling do the default speeds assume?
Carbide inserts — the everyday choice on modern lathes. For HSS tooling, use roughly a third to half of the carbide value: just edit the Vc field.
What feed per revolution should I use?
Roughing: 0.2–0.4 mm/rev. Finishing: 0.05–0.15 mm/rev, where the feed together with the insert's nose radius determines the surface finish. The default 0.2 is a reasonable general-purpose start.
Are these values safe to use directly?
They are starting values for stable setups. Interrupted cuts, long slender parts and parting off warrant slower speeds. Respect your machine's limits and the insert manufacturer's data.
Is my data sent anywhere?
No — this runs entirely in your browser with plain JavaScript. Nothing is uploaded.
What does the coated-insert option do?
Coated inserts allow a higher cutting speed than uncoated carbide — typically +20–50% depending on the coating — +20–50% for TiN and TiCN, and up to +50–100% for TiAlN — but the safe increase in feed rate is much smaller, only about +10–20%, since feed governs chip load and surface finish rather than heat at the cutting edge. This calculator applies a conservative +33% to Vc and +15% to feed per revolution when checked. Treat these as a cautious starting point and verify on your first passes before running faster.
This calculator gives you a starting point — always check it against your machine's real limits and your tool manufacturer's data. Start with a light test pass, then gradually work your way up as you find the sweet spot: quiet running, no vibration, no chatter. Clamp your workpiece securely, and wear the right protective gear — safety glasses, hearing protection, gloves suited to the material, and clothing that won't catch in moving parts.
