Calculating speed and feed in milling differs from turning in two ways: feed is defined per tooth (fz), and cutting speed is calculated not from the nominal tool diameter Dc but from the effective cutting diameter at the actual depth of cut (Dcap). When these two differences are ignored — especially with ball nose and round insert cutters — the calculated spindle speed falls far below the correct value, the tool rubs instead of cutting, and cycle time grows for no reason.
The calculator below produces starting cutting data from the material group and cutter type, and works out the Dcap correction, the average chip thickness hm, the metal removal rate Q and the machining time together.
Milling speed and feed formulas
| Quantity | Formula | Unit |
|---|---|---|
| Spindle speed n | n = (1000 × Vc) / (π × Dcap) | rpm |
| Cutting speed Vc | Vc = (Dcap × π × n) / 1000 | m/min |
| Table feed Vf | Vf = fz × zc × n | mm/min |
| Feed per tooth fz | fz = Vf / (n × zc) | mm/tooth |
| Metal removal rate Q | Q = (ap × ae × Vf) / 1000 | cm³/min |
| Net power Pc | Pc = (ap × ae × Vf × kc) / (60 × 10⁶) | kW |
| Torque Mc | Mc = (Pc × 30 × 10³) / (π × n) | Nm |
| Machining time Tc | Tc = lm / Vf | min |
zc is the number of effective teeth, which is not always the same as the total number of teeth zn. In face milling with a small ae, fewer than one tooth may be engaged at a time, which makes the cut intermittent and increases the risk of vibration. A practical rule: in face milling at least one tooth should always be in cut.
Effective cutting diameter (Dcap): the most common mistake in milling
The diameter in the cutting speed formula is not the nominal diameter of the tool but the largest diameter actually in contact with the workpiece at your chosen depth of cut. With straight cutting edges and a 90° entering angle the two are the same (Dcap = Dc). With ball nose, round insert and angled cutters they are not:
| Cutter type | Effective cutting diameter Dcap |
|---|---|
| Solid end mill, 90° shoulder mill, slot mill | Dcap = Dc |
| Ball nose, ap < Dc/2 | Dcap = 2 × √(ap × (Dc − ap)) |
| Round insert (insert diameter iC) | Dcap = Dc − iC + 2 × √(ap × (iC − ap)) |
| Angled / chamfer mill (Dc measured at the tip) | Dcap = Dc + (2 × ap) / tan κr |
Why it matters. Take a Ø16 mm ball nose cutter machining at 1 mm depth of cut. The effective cutting diameter is Dcap = 2 × √(1 × (16 − 1)) ≈ 7.75 mm, not 16 mm. For Vc 200 m/min the correct spindle speed is 8,220 rpm, but calculating from Dc gives 3,980 rpm — which means the real cutting speed drops to about 97 m/min instead of 200. This is the most common reason why surface quality collapses and tool life comes out far shorter than expected in die and mould machining.
CNC milling speed and feed calculator
Average chip thickness (hm) and the ae/Dc ratio
In milling the cutting edge enters and leaves the workpiece, so chip thickness is not constant: it starts at zero, reaches a maximum and returns to zero. The value that governs cutting force, tool life and power demand is the average chip thickness hm:
hm = (360 × sin κr × ae × fz) / (π × Dcap × arccos(1 − 2ae/Dcap)) (arccos in degrees)
The practical consequence is this: the smaller ae becomes, the thinner the chip. In full slotting (ae = Dc) the average chip thickness is about 0.64 × fz, while at ae = 10% of Dc it drops below 0.2 × fz. If you use the catalog fz value unchanged at small ae, the cutting edge rubs instead of cutting: the edge rounds, heat builds up and tool life falls far below expectation.
The remedy, when ae < Dcap/2, is to raise the feed by the chip thinning correction factor. The calculator above shows this factor and the corrected fz directly. For a full treatment of radial and axial chip thinning and the hex calculation, see Chip formation, chip thinning and maximum chip thickness (h_ex) calculator for CNC milling.
Starting values by cutter type and material
The values below are for starting when you do not have the tool catalog at hand. The definitive value is always the one the cutting tool manufacturer gives for that specific product code.
| Cutter type | Starting fz (mm/tooth) | Effective entering angle κr |
|---|---|---|
| Solid carbide end mill | 0.05 – 0.12 | 90° |
| Indexable 90° shoulder mill | 0.10 – 0.22 | 90° |
| Face mill 45° | 0.15 – 0.30 | 45° |
| Ball nose | 0.06 – 0.15 | depends on ap (variable) |
| Round insert cutter | 0.15 – 0.30 | depends on ap (variable) |
| High feed mill | 0.60 – 1.20 | 10° – 20° |
| Slot mill | 0.04 – 0.09 | 90° |
| ISO material group | Typical Vc in milling (m/min) |
|---|---|
| P — Steel | 150 – 250 |
| M — Stainless steel | 90 – 160 |
| K — Cast iron | 150 – 250 |
| N — Non-ferrous (aluminium, brass) | 300 – 800 |
| S — Titanium / heat resistant alloy | 30 – 80 |
| H — Hardened steel (above 45 HRC) | 50 – 120 |
Choose Vc near the lower end of the range for roughing and near the upper end for finishing. If clamping is weak or the overhang is long, reduce ap and ae first; reducing Vc is usually not the answer, because a very low cutting speed produces built-up edge.
Power, torque and the machine limit in milling
If the values you calculate exceed your machine capacity, the operation will not hold even when the speed and feed are correct. Net power and torque are calculated as:
Pc = (ap × ae × Vf × kc) / (60 × 10⁶) (kW) · Mc = (Pc × 30 × 10³) / (π × n) (Nm)
kc is the specific cutting force and varies with the average chip thickness hm: kc = kc₁ × hm–mc × (1 − γ₀/100). This is why the cutting force per unit area rises in fine machining (small hm) — it is the mathematical expression of why a very small feed is inefficient.
In practice the limit in milling is usually spindle power; but when roughing at low spindle speed with large diameter face mills, torque becomes the limiting factor. For a calculation compared against the machine speed–torque curve, use the CNC spindle torque calculator.
Frequently asked questions
How is spindle speed calculated in milling?
n = (1000 × Vc) / (π × Dcap), where Vc is the cutting speed in m/min and Dcap is the diameter actually cutting at the selected depth of cut. For straight cutting edges with a 90° entering angle Dcap = Dc; for ball nose and round insert cutters Dcap must be calculated separately.
What is the difference between fz and fn?
fz is the feed taken by one tooth in one revolution (mm/tooth). fn is the total feed of the cutter in one revolution: fn = fz × z. Table feed Vf is the distance travelled per minute: Vf = fz × z × n.
Why is the spindle speed different for a ball nose cutter?
Because the full diameter of a ball nose cutter never touches the material. At a shallow depth of cut the engaged diameter is Dcap = 2 × √(ap × (Dc − ap)), which is much smaller than Dc. Spindle speed must be calculated from that smaller diameter, otherwise the real cutting speed stays far below the target.
Should I increase the feed when the radial width of cut ae is small?
Yes. When ae is less than half of Dcap the chip thins out and the catalog fz value produces a chip that is far too thin in practice. The feed must be raised by the chip thinning correction factor; otherwise the cutting edge appears to cut but is in fact rubbing, and it rounds off quickly.