What is the cutting speed formula?

Vc = (D × π × n) / 1000 (m/min). Rearranged for spindle speed: n = (1000 × Vc) / (π × D).

How is the specific cutting force kc calculated?

kc = kc₁ × hm^(–mc) × (1 − γ₀/100) in N/mm², where kc₁ is the specific cutting force at hm = 1 mm, mc a correction factor and γ₀ the rake angle. kc rises as chip thickness falls.

How is the average chip thickness hm found?

In turning with C, D, S, T, V, W insert shapes, hm = fn × sin κr. For round inserts, hm = (360 × fn × ap) / (iC × π × arccos(1 − 2ap/iC)), with arccos in degrees.

What is the spiral cutting length (SCL) used for?

It gives the real distance travelled by the cutting edge in an operation and is used to estimate tool life. In external turning, SCL = (Dm × π / 1000) × (lm / fn) in metres.

How is machining time Tc calculated?

In turning and drilling Tc = lm / (fn × n); in milling Tc = lm / Vf, in minutes, where lm is the machined length.

What do the IT hole tolerance grades mean?

The smaller the IT number the tighter the tolerance, and the tolerance width of a given IT grade increases with diameter. For example, in the Ø18–30 mm range IT7 = 0.021 mm, IT9 = 0.052 mm and IT11 = 0.130 mm.

CNC Machining Formulas and Speed Charts (with Examples)

CNC Machining Formulas, Speed Charts and FAQ: A Worked-Example Reference

Spindle speed, feed, material removal and power formulas for turning, threading, milling and drilling; surface roughness, tolerances and speed charts; worked examples and an FAQ — a Mentor CNC reference guide.

🇹🇷 Bu rehberi Türkçe okuyun

This Mentor CNC reference brings together the most-used CNC machining formulas with worked examples. For tool and parameter selection by material, see the Cutting Tool Selection and Drilling Cutting Parameters guides.

Section 1: Turning Formulas and Worked Examples

Spindle Speed (n / RPM)

n = (V_c × 1000) / (π × D) [rpm]

V_c: cutting speed (m/min), D: workpiece diameter (mm).

Example 1 (P3 steel): V_c 200, D 50 → n = 200000/(π×50) = 1273 rpm.
Example 2 (aluminium): V_c 500, D 80 → n ≈ 2000 rpm.
Example 3 (titanium): V_c 60, D 30 → n ≈ 640 rpm.

Feed Rate (V_f)

V_f = f × n [mm/min]

f: feed (mm/rev).

Steel: n 1273, f 0.15 → V_f = 191 mm/min.
Stainless: n 800, f 0.10 → V_f = 80 mm/min (slow but safe).
Aluminium: n 2000, f 0.30 → V_f = 600 mm/min.

Material Removal Rate (MRR)

Q = V_c × a_p × f [cm³/min]

V_c (m/min), a_p (mm), f (mm/rev). This unit combination gives cm³/min directly; no extra division by 1000.

Fast steel: 300 × 3 × 0.2 = 180 cm³/min.
Fine steel: 180 × 1 × 0.1 = 18 cm³/min.
Aluminium (max efficiency): 500 × 4 × 0.3 = 600 cm³/min.

Net Cutting Power (P_c)

P_c = (V_c × a_p × f × k_c) / (60 × 10³) [kW]

Divisor is 60,000 (60×10³). k_c: specific cutting force (N/mm²). P1≈1800, P3≈2200, M≈2400, K≈1200, N≈600, S≈3000.

⚠ A common power error (fixed)The divisor must be 60×10³ (not 60×10⁴). Example 1: 250×2×0.15×2200/60,000 = 2.75 kW. Example 2 (aggressive): 300×4×0.25×2200/60,000 = 11 kW — near/over the limit of a 5–10 kW machine; reduce a_p or f. Example 3 (titanium): 60×1×0.1×3000/60,000 = 0.3 kW. The source values 0.275 / 1.1 / 0.03 kW were 10× too low.

Section 2: Threading Formulas

Spindle Speed in Threading

n = V_f / P [rpm]

In threading, feed per revolution equals the pitch (V_f = P × n). For a target feed rate: n = V_f / P. The source’s “×1000” version is unnecessary.

M10 × 1.5: V_f 100 mm/min, P 1.5 → n ≈ 67 rpm.
M16 × 2.0: V_f 200, P 2.0 → n = 100 rpm.
M8 × 1.25: V_f 80, P 1.25 → n = 64 rpm.

In practice, speed is usually chosen from diameter and cutting speed (n = V_c×1000/πD); the feed rate then follows as V_f = P × n. Threading is sensitive; vibration control is essential.

Section 3: Milling Formulas and Examples

Cutting Speed (V_c)

V_c = (D_c × π × n) / 1000 ↔ n = (V_c × 1000) / (π × D_c)

D_c: cutter diameter (mm).

Check: Ø20 cutter at 500 rpm → V_c = 20×π×500/1000 = 31 m/min — too low for P3 steel (180–240); raise speed to ≈ 3000 rpm.
Aluminium: Ø16 cutter, V_c 400 → n = 400000/(π×16) ≈ 8000 rpm.

Table Feed (V_f)

V_f = f_z × n × z_n [mm/min]

f_z: feed per tooth (mm/tooth), z_n: number of teeth.

4-tooth (steel): 0.1 × 500 × 4 = 200 mm/min.
3-tooth (stainless): 0.08 × 300 × 3 = 72 mm/min.

Material Removal (Q)

Q = (a_p × a_e × V_f) / 1000 [cm³/min]

a_p: axial depth, a_e: radial width (mm), V_f: feed (mm/min).

Open milling: (5 × 20 × 300)/1000 = 30 cm³/min (fast, efficient).
Narrow milling: (2 × 5 × 100)/1000 = 1 cm³/min (precise, controlled).

Section 4: Drilling Formulas

Cutting Speed / Spindle Speed

V_c = (D_c × π × n)/1000 ↔ n = (V_c × 1000)/(π × D_c)

D_c: drill diameter (mm).

Steel Ø6, V_c 150: n ≈ 8000 rpm.
Aluminium Ø12, V_c 300: n ≈ 8000 rpm.
Stainless Ø8, V_c 70: n ≈ 2800 rpm (slow but normal for stainless).

Feed Rate and Torque

V_f = f × n | M = 9550 × P_c / n [Nm]

Torque: P_c (kW), n (rpm). The source’s “M = P_c×30/(πn)” omitted the kW→W conversion, making it 1000× off.

Standard: f 0.15 × n 8000 = 1200 mm/min. Fine: f 0.08 × n 6000 = 480 mm/min.

Section 5: Surface Roughness (R_a)

Theoretical Roughness (correct form)

R_max ≈ (f² / (8 × r_ε)) × 1000 [µm] | R_a ≈ R_max / 4

f: feed (mm/rev), r_ε: corner radius (mm). Roughness depends on the corner radius, not the workpiece diameter; the source’s diameter-based formula was incorrect.

Practical R_a values (turning)

Feed f	Typical R_a	Class
0.30 mm/rev	3–4 µm	Roughing
0.15 mm/rev	1–2 µm	Medium (H7–H8)
0.08 mm/rev	0.5–1 µm	Finishing

Section 6: Hole/Diameter Tolerances (ISO 286 – IT)

Standard tolerance values (µm)

Size (mm)	IT6	IT7	IT8	IT9	IT10	IT11
3–6	8	12	18	30	48	75
6–10	9	15	22	36	58	90
10–18	11	18	27	43	70	110
18–30	13	21	33	52	84	130
30–50	16	25	39	62	100	160

Practical: H7 for normal production; H8–H9 for wide tolerance; H5–H6 for precision work. Note: the tighter/small-size values in the source table were incorrect; the values above follow ISO 286.

Section 7: Turning Speed Chart

Cutting speed V_c (m/min)

Operation	P1 Steel	P3 Steel	M Stainless	K Cast Iron	N Aluminium	S Titanium
External turning	280–350	200–240	100–150	150–200	400–600	50–80
Boring	250–300	180–200	80–120	120–150	350–500	40–70
Threading	120–160	100–120	50–70	100–140	250–350	30–50
Facing	200–280	150–200	80–120	120–180	400–550	40–70

✓ How to usePick material + operation, take the speed range, compute n = V_c×1000/(πD). Example: P3 external turning, Ø30, V_c 220 → n = 220000/(π×30) ≈ 2333 rpm.

Section 8: Milling Speed Chart

Cutting speed V_c (m/min)

Operation	P1 Steel	P3 Steel	M Stainless	K Cast Iron	N Aluminium
External cut	250–350	180–240	80–120	120–180	350–500
Internal cut	200–280	150–180	60–100	100–150	300–400
Light cut	150–200	100–150	50–80	80–120	200–300
End mill	200–280	120–160	70–100	100–150	300–400

Section 9: Drilling Reference Chart

Material	V_c (m/min)	Feed (mm/rev)	Drill Diameter	Note
P1–P2 Steel	150–200	0.15–0.25	1–20 mm	Use a pilot hole
P3 Steel	120–150	0.12–0.20	1–20 mm	Coolant required
M Stainless	60–80	0.10–0.15	1–15 mm	Very slow
K Cast Iron	100–150	0.15–0.20	1–20 mm	Can run dry
N Aluminium	250–350	0.20–0.35	2–20 mm	High speed

Section 10: Frequently Asked Questions (FAQ)

Turning

Q: My tool wears out after 20 minutes machining P3 steel.
A: Reduce cutting speed by ≈ 15%, check the coolant, and if needed move to a more durable grade (e.g. ceramic/cermet).

Q: There’s a ≈ 0.1 mm deviation on the outer diameter.
A: This is vibration. Check workpiece clamping, holder tightness and tool overhang (shorten it); lower the speed.

Q: The tool breaks in boring.
A: Shorten the tool overhang, reduce speed by ≈ 20% and reduce feed; this operation has the highest vibration risk — take it seriously.

Threading

Q: Chatter appears during threading.
A: Reduce the speed; verify the feed is fully synchronized with the pitch (P); reduce vibration via clamping/machine health.

Q: The thread size is off.
A: Check the machine’s threading/sync mechanism, the pitch (P) setting and the diameter (with a dial indicator).

Milling & Drilling

Q: The milled surface is rough/matte.
A: Reduce feed per tooth (f_z), check tool sharpness, and balance the cutting speed to reduce vibration.

Q: The hole wanders / goes crooked.
A: Use a pilot hole, keep the drill straight and centered, and check part clamping and the symmetry of the drill point.

General

When is coolant a must? Mandatory for steel (P2+), stainless and titanium; optional for cast iron and aluminium.
How do I test parameters? Start low (≈ 70% of the chart value), machine 1–2 min and observe, then ramp up. Cuts easily → +20%; clogs → −20%; breaks → −30%; rough surface → reduce feed.
What if chips aren’t controlled? Long/curled chips wrap the tool, vibration and breakage rise, part and operator are at risk; use a chip-breaker geometry.
When should Mentor CNC parameters be changed? If machine power is insufficient, there is vibration, the tool wears early, surface quality is unacceptable or chip control fails. If all is well, don’t lower them — you’ll reduce efficiency.

Section 11: Setup Checklist

MACHINE [ ] Spindle bearing clean/stable (no vibration) [ ] Tool holder tight [ ] Workpiece clamping secure [ ] Coolant system readyTOOL [ ] Tool sharp and clean [ ] Tool overhang minimal [ ] Dimensions verified with a dial indicatorPARAMETERS [ ] Cutting speed chosen from chart, n computed [ ] Feed set to material [ ] Depth of cut within machine power [ ] First cut 1–2 min: observe [ ] Increased graduallySAFETY [ ] Guard door closed [ ] Hands/accessories clear of the machine [ ] Emergency stop accessible

Conclusion

These formulas and charts are a reference for quickly computing the right speed, feed, removal rate and power. Always verify the values against your own material and machine conditions. For tool selection by material, see the Cutting Tool Selection Guide; for the rest of the series, the Cutting Tools category.

CNC Machining Formulas, Speed Charts and FAQ: A Worked-Example Reference

CNC Machining Formulas, Speed Charts and FAQ: A Worked-Example Reference

Section 1: Turning Formulas and Worked Examples

Section 2: Threading Formulas

Section 3: Milling Formulas and Examples

Section 4: Drilling Formulas

Section 5: Surface Roughness (Ra)

Section 6: Hole/Diameter Tolerances (ISO 286 – IT)

Section 7: Turning Speed Chart

Section 8: Milling Speed Chart

Section 9: Drilling Reference Chart

Section 10: Frequently Asked Questions (FAQ)

Turning

Threading

Milling & Drilling

General

Section 11: Setup Checklist

Conclusion

Related Guides

Questions about CNC, G-code or our calculators? Get in touch.

Section 5: Surface Roughness (R_a)