Spindle speed and feed rate formulas, explained

Spindle speed from cutting speed

Tool makers give a cutting speed: how fast the cutting edge moves across the material, in surface feet per minute (SFM) or metres per minute (vc). The edge of a tool of diameter D travels π × D per revolution, so:

Inch:    RPM = SFM × 12 ÷ (π × D) = 3.82 × SFM ÷ D     (D in inches)
Metric:  n = vc × 1000 ÷ (π × d)                    (vc in m/min, d in mm)

The 3.82 is 12 ÷ π, rounded. For milling and drilling, D is the tool diameter. For turning it is the diameter of the workpiece at the point being cut, which is why constant-surface-speed lathes speed up as a facing cut moves toward the centre.

Feed rate from chip load

Chip load (feed per tooth, IPT or fz) is how thick a bite each cutting edge takes. Multiply it by the number of edges and the speed:

Milling:            IPM = RPM × flutes × chip load      vf = n × z × fz (mm/min)
Turning, drilling:  IPM = RPM × feed per revolution    vf = n × f

Worked example (milling): a 1/2" four-flute carbide end mill in 6061 aluminum at 800 SFM and 0.004" per tooth. RPM = 3.82 × 800 ÷ 0.5 = 6,112. Feed = 6,112 × 4 × 0.004 = 97.79 IPM.

A smaller tool in steel: 1/4" three-flute end mill in 1018 at 400 SFM. RPM = 6,112. Without a catalogue chip load, a common shop starting point is diameter ÷ 200 = 0.00125" per tooth, giving 22.92 IPM. Replace it with the tool maker's value as soon as you have one.

Turning and drilling in metric

Turning a 60 mm steel shaft at the insert maker's 200 m/min: n = 200 × 1000 ÷ (π × 60) = 1,061 1/min. At f = 0.25 mm/rev the carriage moves 265 mm/min.

Drilling an 8.5 mm hole at vc = 80 m/min: n = 2,996 1/min; at 0.15 mm/rev, vf = 449 mm/min.

Turning and drilling speeds depend heavily on the insert grade, coating and coolant, so the calculator asks for the tool maker's vc instead of suggesting one.

Starting cutting speeds for carbide end mills

Coated tools, high-efficiency toolpaths and rigid machines can run well above these numbers; a long-reach tool or a light benchtop mill may need less. The catalogue of the specific tool always wins.

Radial chip thinning

Chip loads in catalogues assume the cutter is engaged at least half its diameter. With a lighter radial step-over, each edge enters the material at a shallow angle and the actual chip comes out thinner than the programmed feed per tooth. Running the catalogue feed at a 10% step-over makes the tool rub instead of cut. The correction raises the feed so the real chip thickness matches the catalogue value:

Adjusted IPT = IPT × D ÷ (2 × √(D × RDOC − RDOC²))      (when RDOC < D ÷ 2)

Example: 1/2" cutter, 0.050" radial depth (10%): factor = 0.5 ÷ (2 × √(0.5 × 0.05 − 0.05²)) = 1.67. A 0.004" catalogue chip load becomes 0.00667" per tooth.

At exactly half the diameter the factor is 1, and above half there is no correction.

When the machine cannot reach the speed

Small tools in aluminum often call for more RPM than the spindle has. Run at the spindle's maximum and recalculate the feed with the same chip load. Example: the 1/2" cutter above wants 6,112 RPM; on a 10,000 RPM spindle that is fine, but a 1/8" cutter at 800 SFM would want 24,448 RPM. At 10,000 RPM with 4 flutes and 0.004" per tooth (if that is the catalogue value for the tool), feed = 10,000 × 4 × 0.004 = 160 IPM, at a lower surface speed than planned.

Do not keep the original feed after capping the speed: the chip load would rise in proportion and can break a small tool.

Metal removal rate

Inch:   MRR (in³/min) = radial width × axial depth × IPM
Metric: Q (cm³/min) = ae × ap × vf ÷ 1000   (ae, ap in mm; vf in mm/min)

For the aluminum example at 0.25" radial width and 0.5" depth: 0.25 × 0.5 × 97.79 = 12.22 in³/min. MRR is useful for comparing strategies and for checking the spindle has the power for the cut.

Common mistakes

• Using the radius instead of the diameter. It doubles the RPM.
• Mixing units: SFM with millimetres, or m/min with inches. Use 3.82 only with inches and SFM.
• Taking the chip load for one diameter and using it on a much smaller tool. Chip load scales roughly with diameter.
• Slowing the feed "to be safe". Too small a chip load rubs, heats the edge and, in stainless steel, work-hardens the surface.
• Ignoring chip thinning on light finishing or adaptive passes.
• For turning, calculating RPM from the stock diameter and forgetting it changes as the part gets smaller.

Questions people ask