Spindle RPM and table feed rate for end mills — set material, cutter diameter, flutes and chip load per tooth.
Start with the end mill supplier’s cutting data for your material, tool diameter, coating and operation. Cutting speed describes how quickly the outside edge travels through the work; spindle speed describes revolutions per minute. The calculator converts between them, then uses flute count and chip load to find table feed. Its presets are broad starting assumptions, so check them against the actual tool before cutting.
RPM = Vc × 1000 / (π × D), where Vc is cutting speed in metres per minute and D is cutter diameter in millimetres. The factor of 1000 converts metres to millimetres. For the same cutting speed, a smaller cutter needs more RPM.
F = RPM × z × fz, where F is table feed in mm/min, z is the number of flutes and fz is chip load in mm per tooth. Milling chip load is per tooth, not per revolution. Feed per revolution equals z × fz.
The values below reproduce this calculator’s HSS presets and 4× carbide assumption in m/min. They are broad workshop estimates, not tool limits or guaranteed recommendations. Alloy grade, cutter coating, engagement and coolant can require different settings; use the manufacturer’s data where available.
| Material | HSS (m/min) | Carbide (m/min) |
|---|---|---|
| Mild steel | 25 | 100 |
| Stainless steel | 12 | 48 |
| Aluminium | 80 | 320 |
| Cast iron | 25 | 100 |
| Brass | 45 | 180 |
Choose fz from the cutter maker’s table for diameter and radial engagement. Small tools and flexible setups generally need lighter loads; larger cutters can often take more. Too little feed can cause rubbing, while excessive load can deflect or break the cutter. Full-width slots need careful chip evacuation and usually different settings from light side milling. Do not apply a thin-chip correction without checking engagement and supplier guidance.
Assume mild steel, Vc = 25 m/min and fz = 0.05 mm/tooth. RPM = 25 × 1000 / (π × 10) ≈ 796. Table feed = 796 × 4 × 0.05 ≈ 159 mm/min. If the machine is set to 800 RPM, use 160 mm/min to preserve the assumed chip load. This illustrates the arithmetic; depth and width of cut still need choosing for your setup.
For other operations, use the lathe turning calculator, tapping speed calculator or drill speed chart.
Does adding flutes increase feed rate?
At the same RPM and chip load, yes: doubling flute count doubles calculated table feed. Check chip space and evacuation, especially when slotting aluminium.
What if my spindle cannot reach the calculated RPM?
Use an available speed appropriate to the tool and recalculate table feed with that actual RPM. Keeping the old feed at a lower RPM increases chip load.
Should I reduce feed if the cutter chatters?
Check workholding, tool overhang, runout and engagement first. Adjust speed or depth of cut as appropriate; simply reducing feed too far can make the cutter rub.