precision_manufacturing Cutting Speed & Feed Calculator (CNC) star

How It's Calculated

Machining reduces to two formulas that scale everything else. Spindle speed converts a material-appropriate cutting speed into an RPM the machine can dial in: n = 1000·Vc ÷ (π·D), where Vc is cutting speed in meters per minute and D is tool (or workpiece) diameter in millimeters. Table feed then converts that RPM into how fast the table should travel: F = n · z · fz, where z is the number of cutting edges (flutes or inserts) and fz is the chip load — how much material each edge shaves off per revolution, in millimeters.

Worked example: a Ø10 mm carbide end mill cutting mild steel at a textbook Vc of 100 m/min gives n = 1000 × 100 ÷ (π × 10) ≈ 3183 RPM. With 4 flutes and a chip load of fz = 0.05 mm, feed becomes F = 3183 × 4 × 0.05 ≈ 637 mm/min. Change any one input — a smaller tool, a tougher material, a different flute count — and both numbers shift together, which is why the calculator exists rather than a lookup chart.

Vc itself always comes from the material and tool combination, never from a universal constant. Typical starting points: HSS on mild steel runs 25-30 m/min; carbide on steel jumps to 80-200 m/min; carbide on aluminum can run 200-500 m/min because aluminum cuts far more freely; stainless with carbide sits lower at 60-120 m/min due to work-hardening and heat retention. These are conservative values meant to be tuned while watching chip color and listening to the cut — the tool manufacturer's own chart for the specific insert grade always outranks a generic number.

What You Should Know

Picking the wrong RPM has real consequences at both extremes, and they are different failure modes, not just "faster is riskier."

• Too slow: the tool rubs rather than shears cleanly, leaving a poor surface finish, work-hardening the material (especially stainless and some aluminum alloys), and stretching cycle time far more than the RPM difference alone suggests.
• Too fast: heat builds up faster than the chip can carry it away, accelerating tool wear, softening the cutting edge, and in the worst case chipping or fracturing the insert. Excess heat can also burn the workpiece surface and, in thin-walled parts, distort dimensions.

The same two formulas apply beyond milling. In turning, D is the workpiece diameter, and since it shrinks as material is removed, RPM should ideally rise through the cut to hold a constant Vc. In drilling, D is the drill diameter and feed is given per revolution rather than per tooth, but n = 1000·Vc/(π·D) is unchanged. If the calculated RPM exceeds the machine's limit, run at its maximum and recompute feed from the achievable RPM — never keep the original feed at a reduced RPM, since that overloads each tooth.