Milling speed & feed calculator
Spindle speed from cutter diameter and material, table feed from your chip load — the two numbers every milling job starts with.
Getting speed and feed right the first time
The number a cutting tool actually cares about is not rpm — it is cutting speed, the speed at which the edge travels through the material, measured in metres per minute. Every material has a range it likes: run below it and the tool rubs instead of cutting, run above it and the edge overheats and dulls in seconds. Because the same rpm gives a completely different cutting speed on a 3 mm cutter than on a 20 mm one, rpm on its own is meaningless. That is what this calculator does: you give it the material and the diameter, and it works back to the spindle speed that puts the edge in the right range.
From cutting speed to spindle speed
The formula is n = (Vc × 1000) / (π × Ø), where n is the spindle speed in rpm, Vc the cutting speed in m/min and Ø the cutter diameter in mm. The practical consequence is worth internalising: halve the diameter and you double the rpm. That is why small cutters scream and large ones turn slowly, and why a 3 mm end mill in aluminium genuinely wants around 18 000 rpm — a number that looks alarming until you realise the edge is only travelling about 170 m/min. Both the Vc field and the rpm field can be edited here, so you can work either way: start from a material and get the speed, or type the maximum rpm your machine can reach and see what cutting speed that leaves you.
Chip load, the number most people guess at
Spindle speed alone does not tell you how fast to move. That is the feed: Vf = fz × z × n, where fz is the chip each tooth takes and z the number of teeth. Getting this wrong is more damaging than getting rpm wrong. Feed too slowly and the tooth rubs rather than cuts, which generates heat, work-hardens the surface and kills the edge; feed too fast and you overload the tooth and break it. As a rough guide, fz is roughly 0.5 to 1% of the cutter diameter — about 0.03 to 0.06 mm per tooth on a 6 mm end mill. Manufacturers publish exact values for their own tools, and those always win over any rule of thumb.
What a coating actually buys you
A coated cutter tolerates more heat, which means more speed and more feed. Real-world figures vary by coating and material: roughly +20 to 50% for TiN, +30 to 50% for TiCN, and +50 to 100% for TiAlN. This calculator deliberately applies a conservative +33% to both the cutting speed and the chip load when you tick the box — the middle of that range rather than the top of it. That is a starting bump, not a promise. Take the first cuts with a newly coated tool gently and confirm the numbers hold in your setup before pushing further.
When to back off from the calculated numbers
These are starting values for a rigid setup with cooling, and rigidity is the assumption that breaks first. Reduce speed and feed when the cutter hangs a long way out of the holder, when you are cutting a deep slot where chips struggle to escape, when the workpiece is a thin wall that can flex, or when the part is held in anything less than a solid clamp. The clearest signal is sound: a cut that is working sounds steady, and one that chatters is telling you something is moving that should not be. Chatter is usually cured by taking a lighter cut or shortening the tool, not by slowing down alone.
Metric and imperial, and where the numbers came from
The unit button converts every field and label between metric and imperial — millimetres and inches, m/min and SFM, mm/tooth and inch/tooth. The calculation itself always runs in metric internally, so switching units never changes a result, only how it is written. The material table and cutting speeds behind this calculator come from a workshop tool built for real production use rather than copied from a supplier catalogue, and they are calibrated against a known reference point. They remain starting values: your machine, your holder and your material batch all have a vote.
Speed and feed belong together
The spindle speed comes from the cutting speed and the cutter diameter: n = (Vc × 1000) / (π × Ø). But rpm alone says nothing about how fast to move the table — that's the feed: Vf = fz × z × n, where fz is how thick a chip each tooth takes and z the number of teeth. Spinning fast while feeding too slowly rubs and burns the cutter; feeding too fast overloads it. The pair is what matters.
Which tooling do the default speeds assume?
Solid carbide end mills — calibrated against a real reference point (aluminium, 3 mm end mill at 18 000 rpm ≈ Vc 170 m/min). For HSS cutters, roughly halve the cutting speed: just edit the Vc field.
What chip load (fz) should I use?
Small cutters take small chips: as a rough guide, fz ≈ 0.5–1% of the cutter diameter (a 6 mm end mill: 0.03–0.06 mm per tooth). Manufacturers publish exact values per cutter — those always win.
Are these values safe to use directly?
They are starting values for rigid setups with cooling. Long overhangs, deep slots and thin walls warrant slower, lighter cuts. Respect your machine's spindle and feed limits.
Is my data sent anywhere?
No — this runs entirely in your browser with plain JavaScript. Nothing is uploaded.
What does the coated-cutter option do?
Coated end mills tolerate higher speeds and feeds — roughly +20–50% for TiN, +30–50% for TiCN, and +50–100% for TiAlN, depending on the coating and material. This calculator conservatively applies +33% to both Vc and feed per tooth (fz) when checked — a safe starting bump, not a guarantee. Take it easy on your first cuts with a newly coated tool to confirm the numbers hold before pushing further.
Ball nose and tapered mills — why the different speed?
With a flat end mill the whole diameter cuts, so the nominal Ø sets the speed. A ball nose only reaches its full diameter at half its radius deep — shallower than that, the cut happens on a smaller effective diameter, so the calculator raises the spindle speed to keep the same cutting speed where the tool actually cuts. Enter your depth of cut and it shows the effective Ø and the compensated rpm. A tapered mill changes diameter along its length, so give the depth of cut and the taper's half-angle and it uses the diameter at that point. These are starting figures — check them against your setup, and go gently on the first pass.
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.
