Cutting Speed

In plain English

Cutting speed is how fast the edge of the tool travels across the material — like the speed of a car, measured in metres per minute. Every combination of tool and material has a comfortable cutting speed: too slow wastes time and can give a poor finish; too fast overheats and wears out the tool quickly. The machine, however, is set in revolutions per minute, so you convert between the two using the diameter.

Technical definition

Cutting speed V_c is the instantaneous velocity of the cutting edge relative to the workpiece in the primary direction of motion. In turning it is the surface speed of the workpiece at the diameter being cut; in milling and drilling it is the peripheral speed of the tool. It is expressed in m/min (metric) or surface feet per minute, SFM (inch).

How it works and where it is used

Tool suppliers publish recommended cutting speeds for each tool grade and work-material group, often with a range depending on feed and depth of cut. You choose a speed from that data, then calculate the spindle RPM. Because speed depends on diameter, the RPM must be higher for small diameters and lower for large ones. CNC lathes can keep cutting speed constant (constant surface speed, G96) as the diameter changes, within a programmed RPM limit.

Formula

V_c = π × D × n ÷ 1000    n = 1000 × V_c ÷ (π × D)

Inch: n = 12 × SFM ÷ (π × D)

V_c = cutting speed (m/min), D = workpiece diameter in turning or tool diameter in milling/drilling (mm; inches in the inch form), n = spindle speed (rpm).

Worked example

Turning a 50 mm bar at a recommended 120 m/min: n = 1000 × 120 ÷ (π × 50) = 764 rpm. A 10 mm drill at 25 m/min: n = 1000 × 25 ÷ (π × 10) = 796 rpm. In inch units, 400 SFM on a 2 in bar: n = 12 × 400 ÷ (π × 2) = 764 rpm.

In the workshop and in practice

Cutting speed has the largest effect of all cutting data on tool life (see tool life). On manual machines, set the nearest available spindle speed below the calculated value. When facing towards the centre, cutting speed falls to zero at the axis even at full RPM — another reason CNC lathes use constant surface speed with a maximum RPM clamp.

Common mistakes and misconceptions

• Using the tool diameter in turning. In turning, use the workpiece diameter being cut.
• Confusing cutting speed with feed rate. Feed is how far the tool advances per revolution or per tooth; it is set separately.
• Copying speeds between materials. A speed suitable for aluminium is far too high for stainless steel or titanium.
• Exceeding the chuck or spindle limit. Small diameters at high cutting speed can call for more RPM than is safe.

Related calculators

• Cutting Speed & Spindle RPM Calculator — Spindle speed from cutting speed and diameter — or cutting speed from RPM.
• Lathe Turning Time Calculator — Machining time for a turning operation from length, feed and RPM or cutting speed.
• Taylor Tool Life Calculator — Tool life from cutting speed with V·Tⁿ = C, the speed for a target life, or n and C from two tests.
• Turning Material Removal Rate Calculator — Metal removal rate (cm³/min) of a turning cut from diameter, depth of cut, feed and speed.

Related topics

• Tool Life — How long a cutting edge lasts before it must be changed, and how speed controls it.
• Torque — The turning effect of a force about an axis — force times lever arm.

References

• ISO 3002-3: Basic quantities in cutting and grinding — Part 3: Geometric and kinematic quantities in cutting (cutting speed and feed)
• Kalpakjian and Schmid, Manufacturing Engineering and Technology (machining fundamentals)
• Machinery’s Handbook (Industrial Press), speeds and feeds