Formulas for Turning Milling: A Working Reference for the Shop Floor

• 1
  Cutting speed: the base number behind formulas for turning milling
• 2
  Feed per tooth and feed per revolution
• 3
  Metal removal rate tells you what the cycle will cost
• 4
  Cutting power and torque: where the setup breaks
• 5
  When the formulas stop being right
• 6
  Which formula to use for which operation

Almost every parameter argument on a shop floor starts with surface speed. It decides how much heat the edge sees and how fast the coating wears. The formula is short: vc = π × D × n ÷ 1000, with vc in m/min, D in mm and n in rpm. Rearranged for the machine, n = 1000 × vc ÷ (π × D).

For a Ø50 mm 6061-T6 face mill at vc = 400 m/min, n works out to about 2,550 rpm. Drop to a Ø10 mm end mill at the same vc and n jumps to roughly 12,700 rpm, which many spindles cannot reach. That is the trap. Surface speed stays constant while rpm scales inversely with diameter, so small tools often run below the ideal cutting speed and rub instead of cut.

The same logic applies to drilling and boring. A Ø8 mm drill in 304 stainless at vc = 25 m/min needs only about 1,000 rpm, while a Ø25 mm boring bar at the same vc needs roughly 320 rpm. Boring is where the formula pays off most, because bar deflection grows with overhang and the operator is usually trading speed for rigidity.

Treat vc as a range, not a single value. Carbide in aluminum sits around 300–600 m/min, in mild steel 150–250 m/min, in 304 stainless 120–180 m/min, and in titanium 40–80 m/min. HSS tools run about one third of those figures. Start at the low end when the setup is weak, when the part is thin-walled, or when the tool has long overhang.

• 1
  vc = π × D × n ÷ 1000Solve for n when setting spindle speed.
• 2
  n = 1000 × vc ÷ (π × D)Small diameter means high rpm; check spindle limit.
• 3
  vc ranges by materialAluminum 300–600 m/min, 304 stainless 120–180 m/min, titanium 40–80 m/min.

Speed sets heat; feed sets chip thickness. Chip thickness is what actually breaks the material ahead of the edge. Too thin and the tool rubs, work-hardens the surface and wears fast. Too thick and you overload the edge or pull the part out of the vise.

For milling, feed rate is vf = fz × z × n, where fz is feed per tooth, z is the number of flutes and n is rpm. A 4-flute Ø12 mm carbide end mill at fz = 0.05 mm and n = 8,000 rpm gives vf = 1,600 mm/min. Halve the flute count and you halve the table feed if fz stays the same. This is why aluminum jobs often run 3-flute cutters: more chip room per flute, so you can push fz higher.

For turning, the equivalent is feed per revolution, fn in mm/rev. It has a direct effect on surface finish. The theoretical roughness is close to Ra ≈ fn² × 1000 ÷ (32 × r), where r is the tool nose radius in mm. With fn = 0.2 mm/rev and r = 0.8 mm, Ra lands near 1.6 μm. Push fn to 0.3 mm/rev and Ra roughly doubles. That is the trade: cycle time against finish.

For drilling, feed per revolution is usually the parameter on the drill data sheet, often 0.05–0.15 mm/rev for general steel and 0.15–0.3 mm/rev for aluminum. Boring uses the same turning formula, but the limiting factor is usually chatter rather than edge load. When a boring bar sings, reduce fn before you reduce depth of cut.

• 1
  vf = fz × z × nMilling table feed from feed per tooth.
• 2
  Ra ≈ fn² × 1000 ÷ (32 × r)Turning finish estimate from feed and nose radius.
• 3
  fc = fn × ap × vc ÷ 60Chip load check in cm³/min per unit time.

Metal removal rate, MRR, is the volume of material taken off per minute. It is the fastest way to compare two process plans before you cut metal. For milling, MRR = ap × ae × vf ÷ 1000, with axial depth ap and radial width ae in mm and vf in mm/min, giving cm³/min.

A Ø16 mm end mill at ap = 3 mm, ae = 8 mm, vf = 2,000 mm/min removes 48 cm³/min. The same cutter in a full-width slot at ae = 16 mm and half the feed removes the same volume but puts far more load on the tool and spindle. High-efficiency milling flips this: shallow ap, wide ae, high vf, lower radial engagement per tooth.

Turning uses MRR = ap × fn × vc × 1000 ÷ 1000, which simplifies to ap × fn × vc in cm³/min when ap is in mm, fn in mm/rev and vc in m/min. Drilling is close to MRR = π × D² ÷ 4 × fn × n ÷ 1000. Boring follows the turning form with the bore diameter rather than the outside diameter.

MRR is a planning number, not a target. If the machine cannot deliver the spindle power or the fixture cannot hold the part, the calculated MRR is fiction. Use it to compare options, then confirm against spindle load on the first part.

• 1
  Milling: ap × ae × vf ÷ 1000Axial and radial depth times table feed.
• 2
  Turning: ap × fn × vcClose approximation in cm³/min.
• 3
  Drilling: π × D² ÷ 4 × fn × n ÷ 1000Bore area times feed per rev times rpm.

Power is the check that stops you from stalling the spindle. Net cutting power Pc = ap × ae × vf × kc ÷ (60 × 10⁶), with kc the specific cutting force in N/mm², giving kW. For 6061 aluminum kc is roughly 700 N/mm², for mild steel about 1,800 N/mm², for 304 stainless near 2,300 N/mm² and for titanium around 2,000–2,500 N/mm².

A 48 cm³/min cut in 304 stainless needs about 1.8 kW at the tool, before spindle and drive losses. Add 20–30 percent for machine efficiency and you are near 2.3 kW. That is fine on a 15 kW spindle but marginal on a small benchtop machine. The formula is doing its job: it flags the risk before the tool squeals.

Torque matters more than power on low-rpm work. Mc = Pc × 9,550 ÷ n, in N·m, with Pc in kW and n in rpm. A Ø60 mm boring head at 200 rpm and 5 kW of cutting power needs roughly 240 N·m, which many lathes cannot hold. This is why large-diameter boring often runs at a conservative feed and depth.

k c values are approximate. They shift with hardness, microstructure and rake angle, and they rise as chip thickness falls below about 0.05 mm because of edge ploughing. When the number on the spindle load meter reads 20 percent above your calculation, the material is harder than the data sheet assumed.

• 1
  Pc = ap × ae × vf × kc ÷ (60 × 10⁶)Net cutting power at the tool, in kW.
• 2
  Mc = Pc × 9,550 ÷ nTorque check for low-rpm, large-diameter work.
• 3
  kc by materialAluminum ~700, mild steel ~1,800, stainless ~2,300 N/mm².

Every formula on this page assumes a rigid setup, a sharp edge and a stable chip. Break any of those and the arithmetic drifts away from reality. The most common failure is chatter. Chatter is a vibration problem, not a cutting-force problem, so reducing feed or depth is often more effective than recalculating speed.

Long overhang is the second limit. A boring bar at 4:1 length-to-diameter is predictable; at 8:1 the static formulas underestimate deflection and the bar starts to bend under load. Tool runout is the third. A 0.02 mm runout on a 4-flute cutter means one flute carries most of the load, so the calculated fz is not what the edge actually sees.

Material condition also matters. A 6061-T6 casting and a 6061-T6 extrusion share a data sheet but not a chip. Work-hardened 304 can push kc well above the nominal value. Heat-treated 4140 at 30 HRC cuts differently from the same steel in the annealed state.

Use the numbers as a starting point, then listen, look at the chip and read the load meter. The formulas explain why a cut works. They do not replace the first part.