Skip to content
Guides

CNC speeds and feeds: spindle rpm, feed rate and cutting power

How to calculate CNC speeds and feeds: spindle rpm from cutting speed, feed rate from chip load, metal removal rate, chip thinning and cutting power, with a worked 16 mm end mill example in mild steel.

By Site AdministratorUpdated 9 min read

Every milling job starts with the same questions: how fast should the spindle turn, how fast should the table feed, and will the machine have enough power for the cut? The tool maker gives you a cutting speed and a feed per tooth. Turning those into spindle rpm, feed rate, metal removal rate and cutting power is the CNC speeds and feeds calculation, and it takes five short formulas. This guide works through them in order, explains chip thinning (the reason light radial cuts can run faster feeds), and finishes with a fully worked example for a 16 mm carbide end mill in mild steel.

Top view of a 16 mm, 4-flute end mill side milling a steel block with 4 mm radial width of cut and 12 mm axial depth, engagement angle 60 degrees, with the speed and feed formulas and results: 2,984 rpm, 597 mm/min feed, 28.6 cm³/min metal removal and 1.41 kW cutting power

The numbers you need before you start

  • Cutting speed Vc (m/min or SFM): the surface speed at the cutting edge. It comes from the tool maker's catalogue for your tool grade and work material.
  • Cutter diameter D (mm or inch) and number of teeth (flutes) z.
  • Feed per tooth fz (mm or inch): the chip load each tooth takes, also from the catalogue.
  • Axial depth of cut ap and radial width of cut ae (mm): how deep along the tool axis and how wide into the side of the part the cutter engages.
  • For the power check: the specific cutting force of the material (kc1 and mc) and the spindle's power and speed range.

Step 1: spindle speed from cutting speed

The cutting speed is the distance a point on the cutting edge travels per minute. One revolution moves it π × D, so:

n = (1000 × Vc) / (π × D)

  • n = spindle speed, rpm
  • Vc = cutting speed, m/min
  • D = cutter diameter, mm (the factor 1000 converts metres to millimetres)

In inch units the same formula becomes rpm = (SFM × 3.82) / D, with D in inches; 3.82 is 12/π. A 16 mm cutter at 150 m/min runs at 1000 × 150 / (π × 16) = 2,984 rpm. If the result is above the spindle's maximum speed, the machine runs at its limit, and the feed rate in the next step must be recalculated from the speed it actually runs at.

Step 2: feed rate from feed per tooth

Each tooth removes a chip of thickness fz per revolution, so the table feed is:

vf = fz × z × n

vf is in mm/min when fz is in mm. In inch units, IPM = chip load × flutes × rpm. For the 16 mm, 4-flute cutter at 0.05 mm per tooth and 2,984 rpm: vf = 0.05 × 4 × 2,984 = 597 mm/min (23.5 in/min). Feed per revolution, fn = fz × z, is 0.20 mm.

Step 3: metal removal rate

The metal removal rate Q is the volume of chips made per minute. It is the best single number for comparing strategies:

Q = (ap × ae × vf) / 1000

Q is in cm³/min with ap, ae in mm and vf in mm/min. With ap = 12 mm and ae = 4 mm at 597 mm/min, Q = 12 × 4 × 597 / 1000 = 28.6 cm³/min. Power is roughly proportional to Q, which is why the next two steps matter.

Step 4: chip thickness and chip thinning

The catalogue feed per tooth assumes the tooth reaches the full chip thickness fz at some point in its path. That happens only when the radial width of cut is at least half the cutter diameter. With a narrower cut the tooth leaves the material before the chip gets that thick, so the real chip is thinner than fz. This is radial chip thinning.

Engagement angle and maximum chip thickness

For side milling with a straight-edged cutter, the angle through which each tooth stays in the cut is:

φ = arccos(1 − 2 × ae / D)

and, while ae is less than D/2, the maximum chip thickness is:

hex = fz × sin φ

With ae = 4 mm on a 16 mm cutter, ae/D = 0.25, φ = arccos(0.5) = 60° and hex = 0.05 × 0.866 = 0.043 mm. If the tool maker's 0.05 mm is meant as the chip thickness the edge should see, the programmed feed per tooth can be raised to fz = hex / sin φ = 0.05 / 0.866 = 0.058 mm. At very light cuts the correction is large: at ae/D = 0.05 the feed can be more than doubled. Many catalogues already include this correction in their tables, so check before applying it twice.

Bar chart of the chip thinning factor, programmed feed per tooth divided by maximum chip thickness, against radial width of cut: 1.00 at ae/D 0.5, 1.15 at 0.25, 1.67 at 0.10 and 2.29 at 0.05, with engagement angles 90, 60, 36.9 and 25.8 degrees

Average chip thickness

The cutting force depends on the average chip thickness over the engagement arc. For a cutter with a 90° entering angle:

hm = (360 × fz × ae) / (π × D × φ), with φ in degrees

For the example, hm = 360 × 0.05 × 4 / (π × 16 × 60) = 0.0239 mm. For cutters with a smaller entering angle κr (for example 45° face mills), multiply by sin κr.

Step 5: cutting power and spindle torque

The force needed to cut a chip of cross-section 1 mm² is the specific cutting force kc. It rises as the chip gets thinner, which is described by:

kc = kc1 × hm^(−mc)

kc1 is the specific cutting force for a chip 1 mm thick and mc is the material's chip-thickness exponent. The net cutting power at the tool is then:

Pc = (ap × ae × vf × kc) / (60 × 10⁶)

Pc is in kW with ap, ae in mm, vf in mm/min and kc in N/mm². Divide by the efficiency of the spindle drive (often taken as about 0.8 for planning) to get the spindle power required, and check the torque at the speed you are running:

T = 9549 × Pc / n (N·m, with Pc in kW)

Typical starting values for kc1 and mc, from a tool maker's material group table (ISO 513 groups), are listed below. Values for a particular grade and tool geometry vary, and a positive rake angle lowers kc, so use your own tool maker's data where you have it.

Material (ISO group)
kc1 (N/mm²)
mc
Non-alloy steel, below 0.25% C, annealed (P)
1,350
0.21
High-alloy and tool steel, annealed (P)
2,450
0.23
Ferritic or martensitic stainless steel (M)
1,875
0.21
Austenitic or duplex stainless steel (M)
2,150
0.20
Grey cast iron (K)
1,150 to 1,350
0.20 to 0.28
Wrought aluminium, not hardenable (N)
700
0.25
Wrought aluminium, hardenable (N)
800
0.25

Worked example: CNC speeds and feeds calculation for a 16 mm end mill in mild steel

A 16 mm solid carbide end mill with 4 flutes is side milling a low-carbon steel part. The catalogue recommends Vc = 150 m/min and fz = 0.05 mm. The cut is ap = 12 mm deep and ae = 4 mm wide. The material is taken as kc1 = 1,350 N/mm², mc = 0.21.

1. Spindle speed: n = 1000 × 150 / (π × 16) = 2,984 rpm.

2. Feed rate: vf = 0.05 × 4 × 2,984 = 597 mm/min.

3. Metal removal rate: Q = 12 × 4 × 597 / 1000 = 28.6 cm³/min.

4. Chip thickness: ae/D = 0.25, φ = 60°, hex = 0.043 mm, hm = 0.0239 mm.

5. Specific cutting force: kc = 1,350 × 0.0239^(−0.21) ≈ 2,958 N/mm². The thin chip roughly doubles kc compared with kc1.

6. Cutting power: Pc = 12 × 4 × 597 × 2,958 / (60 × 10⁶) = 1.41 kW (1.89 hp).

7. Spindle power and torque: 1.41 / 0.8 ≈ 1.77 kW at the motor; torque T = 9549 × 1.41 / 2,984 ≈ 4.5 N·m.

If the tool maker's 0.05 mm is a target chip thickness, chip thinning allows fz = 0.058 mm. The feed then rises to 689 mm/min, Q to 33.1 cm³/min and the cutting power to about 1.58 kW (about 1.98 kW at the spindle): 15% more output for the same chip load on the edge. A small machining centre with a 5.5 kW spindle has plenty of margin for either setting; a light hobby machine with a 0.8 kW spindle would not, and would need a smaller ap or ae.

The same example in inch units: 16 mm = 0.63 in and 150 m/min = 492 SFM, so rpm = 492 × 3.82 / 0.63 ≈ 2,984; chip load 0.002 in × 4 flutes × 2,984 rpm ≈ 23.5 in/min; Q ≈ 1.75 in³/min.

Turning uses the same ideas

On a lathe the diameter in the speed formula is the workpiece diameter, and the feed is given per revolution:

  • Spindle speed: n = 1000 × Vc / (π × Dm)
  • Feed rate: vf = fn × n
  • Metal removal rate: Q = Vc × ap × fn (cm³/min)
  • Net power: Pc = Vc × ap × fn × kc / (60 × 10³) (kW), with chip thickness hm ≈ fn × sin κr

Turning a 60 mm steel bar at 180 m/min with fn = 0.25 mm and ap = 2 mm (κr = 90°): n = 955 rpm, vf = 239 mm/min, Q = 90 cm³/min, kc = 1,350 × 0.25^(−0.21) ≈ 1,806 N/mm² and Pc ≈ 2.71 kW, or about 3.4 kW at the spindle. As the diameter shrinks the rpm must rise to keep the cutting speed, which is what constant surface speed (G96) does on a CNC lathe.

Common mistakes in speed and feed calculations

  • Mixing inch and metric. SFM with a diameter in millimetres, or a chip load in inches with a feed in mm/min, gives answers out by a factor of 25.4 or 3.28. Our article on unit mistakes that cost money lists the usual traps.
  • Using the shank diameter instead of the cutting diameter. For ball-nose cutters at shallow depth and for chamfer tools, the effective cutting diameter is smaller than the nominal size, so the real cutting speed is lower than you think.
  • Ignoring the spindle limit. If the calculated rpm is above the machine's maximum, recalculate the feed from the speed the spindle can really reach, or the chip load will be too high.
  • Feeding too lightly. A chip that is too thin rubs instead of cutting, which work-hardens stainless steel and wears the edge quickly. Check hex, not just fz.
  • Checking power but not torque. Large face mills and taps run at low rpm, where many spindles cannot deliver their rated power. Compare the torque from Step 5 with the spindle's torque curve.

Quick reference

  • Spindle speed: n = 1000 × Vc / (π × D); rpm = SFM × 3.82 / D(in)
  • Feed rate: vf = fz × z × n
  • Metal removal rate: Q = ap × ae × vf / 1000 (cm³/min)
  • Engagement angle: φ = arccos(1 − 2ae/D); hex = fz × sin φ when ae < D/2
  • Average chip thickness: hm = 360 × fz × ae / (π × D × φ°)
  • Specific cutting force: kc = kc1 × hm^(−mc)
  • Cutting power: Pc = ap × ae × vf × kc / (60 × 10⁶) kW; spindle power = Pc / η
  • Torque: T = 9549 × Pc / n (N·m)

To run these numbers for your own tools, use the CNC speed and feed calculator, which returns rpm, feed rate, metal removal rate and cutting power in one step. To pick a motor and reduction for a machine drive, see the motor and drive calculator and our guide to choosing a motor and gearbox from power and speed. The unit converter handles SFM, in/min and hp. For background on the terms, see Speeds and feeds (Wikipedia).

#spindle speed#metal removal rate#milling#speeds and feeds#CNC#feed rate#cutting power

Keep reading