CNC Cutting Speed and Feed Rate: Complete Calculation Guide for Machinists
Correct cutting speed and feed rate are the two most important variables in CNC machining. Too fast and the tool breaks; too slow and you waste cycle time. This guide covers the exact formulas, reference tables for common materials, and worked examples for both turning and milling.
Cutting speed (also called surface speed) and feed rate are the two fundamental parameters that govern every CNC turning and milling operation. Getting them right maximises tool life, ensures dimensional accuracy, achieves the required surface finish, and minimises cycle time.
The problem is that these two parameters interact with each other and with dozens of other variables: workpiece material, tool material, tool geometry, depth of cut, coolant, machine rigidity, and workholding stiffness. This guide provides the formulas, reference tables, and worked examples you need to establish a safe starting point and refine from there.
Cutting Speed vs. Feed Rate — The Key Distinction
These terms are often confused, so it is worth being precise:
Surface Speed (Vc): The speed at which the cutting edge moves relative to the workpiece, measured in metres per minute (m/min) or surface feet per minute (SFM). Surface speed depends on the material being cut and the tool material — it is the primary driver of tool temperature and tool wear.
Spindle Speed (n): The rotational speed of the spindle in RPM. For a given surface speed and tool diameter, there is exactly one correct RPM. This is what you actually enter into the CNC controller.
Feed Rate (f): For turning, feed rate is the distance the tool advances per revolution of the workpiece (mm/rev). For milling, it is usually expressed as feed per tooth (chip load, mm/tooth) and converted to a table feed rate (mm/min). Feed rate controls chip thickness, cutting forces, and surface finish.
RPM Formula
n (RPM) = (1000 × Vc) ÷ (π × D)
Where: n = Spindle speed (RPM) Vc = Recommended cutting speed (m/min) D = Cutting diameter (mm) — workpiece diameter for turning, tool diameter for milling π = 3.14159
For SFM input: n (RPM) = (12 × SFM) ÷ (π × D_inches)
Example (turning): Turning 304 stainless steel with a carbide insert. Recommended Vc = 180 m/min. Workpiece diameter = 75 mm. n = (1000 × 180) ÷ (3.14159 × 75) = 180,000 ÷ 235.6 = 764 RPM
Milling Table Feed Rate Formula
For milling operations, the table feed rate is calculated from the chip load per tooth:
Vf (mm/min) = n × fz × z
Where: Vf = Table feed rate (mm/min) n = Spindle speed (RPM) fz = Chip load per tooth (mm/tooth) z = Number of flutes (teeth) on the milling cutter
Example (milling): End milling 6061 aluminium with a 12 mm diameter, 4-flute carbide end mill. Recommended Vc = 300 m/min, chip load = 0.05 mm/tooth. n = (1000 × 300) ÷ (3.14159 × 12) = 300,000 ÷ 37.7 = 7,958 RPM Vf = 7,958 × 0.05 × 4 = 1,592 mm/min
Recommended Cutting Speeds by Material
These are starting-point surface speeds for carbide tooling. Reduce by 40-60% for high-speed steel (HSS) tooling. Values represent continuous cutting in dry or flood coolant conditions.
| Material | Vc Turning (m/min) | Vc Milling (m/min) | Notes |
|---|---|---|---|
| 6061 Aluminium | 250–600 | 200–500 | High speeds acceptable; watch for built-up edge at low speeds |
| 1018 Mild Steel | 150–250 | 100–200 | Good machinability; use flood coolant |
| 4140 Alloy Steel (HT) | 80–150 | 60–120 | Harder material; sharp inserts essential |
| 304 Stainless Steel | 120–200 | 80–150 | Work-hardens rapidly; maintain feed rate |
| 316L Stainless Steel | 100–180 | 70–130 | More gummy than 304; sharp, positive rake tools |
| Titanium Ti-6Al-4V | 40–80 | 30–60 | Very low thermal conductivity; flood coolant critical |
| Inconel 718 | 20–45 | 15–35 | Super-alloy; specialised inserts, heavy coolant |
| Cast Iron (grey) | 100–200 | 80–160 | Dry cutting acceptable; abrasive on tool flank |
| Copper / Brass | 200–400 | 150–300 | Gummy; positive rake tooling, no coolant often preferred |
| HDPE / Nylon | 200–500 | 150–400 | Sharp HSS or carbide; clear chips frequently |
Recommended Chip Loads for Milling
Chip load (fz) depends on tool diameter, tool material, and workpiece material. These values are for solid carbide end mills.
| Tool Dia (mm) | Aluminium fz (mm) | Steel (mild) fz (mm) | Stainless fz (mm) | Titanium fz (mm) |
|---|---|---|---|---|
| 4 | 0.020–0.030 | 0.010–0.015 | 0.008–0.012 | 0.005–0.008 |
| 6 | 0.030–0.050 | 0.015–0.025 | 0.012–0.018 | 0.008–0.012 |
| 10 | 0.040–0.070 | 0.020–0.035 | 0.016–0.025 | 0.010–0.016 |
| 12 | 0.050–0.080 | 0.025–0.040 | 0.020–0.030 | 0.012–0.020 |
| 16 | 0.060–0.100 | 0.030–0.050 | 0.025–0.038 | 0.015–0.025 |
| 20 | 0.080–0.130 | 0.035–0.060 | 0.030–0.045 | 0.018–0.030 |
Depth of Cut Recommendations
Axial Depth of Cut (ap) — also called depth of cut in turning or axial depth (ADOC) in milling — is how deep the tool engages in the axial direction.
Radial Depth of Cut (ae) — in milling only — is how wide the tool engages radially. Expressed as a percentage of tool diameter.
For roughing, maximise material removal rate (MRR): MRR (cm³/min) = ap (mm) × ae (mm) × Vf (mm/min) ÷ 1000
For finishing, prioritise surface finish. Use: - ap = 0.1–0.3 mm - ae = 5–15% of tool diameter - Increase Vc by 20–30% above roughing speed - Consider a wiper insert or multi-flute tool for better Ra
Turning depth of cut: Roughing 1–5 mm, Finishing 0.1–0.5 mm.
Tool Life and Taylor's Equation
Taylor's tool life equation quantifies how cutting speed affects tool life:
Vc × T^n = C
Where: Vc = Cutting speed (m/min) T = Tool life (minutes) n = Taylor exponent (material/tool dependent, typically 0.1–0.4) C = Taylor constant (cutting speed for 1-minute tool life)
For carbide on steel, n ≈ 0.25. This means doubling the cutting speed reduces tool life to about 1/16th of its original value. This is why exceeding recommended speeds by even 20% can halve tool life.
Practical implication: If you are running at the high end of the recommended speed range and experiencing premature tool wear, reducing Vc by 15% will approximately double tool life — a worthwhile trade-off for long-run production.
Troubleshooting Common Problems
Use the following table to diagnose machining problems and adjust parameters:
| Symptom | Likely Cause | Adjustment |
|---|---|---|
| Tool chipping | Feed rate too high; interrupted cut | Reduce fz by 20%; check for vibration |
| Flank wear too rapid | Vc too high | Reduce surface speed by 15–20% |
| Built-up edge (BUE) | Vc too low; wrong tool geometry | Increase Vc; use positive rake insert |
| Poor surface finish | Too high feed; too large ap; vibration | Reduce feed; check tool runout; improve fixturing |
| Tool deflection / chatter | Long overhang; high radial force | Shorten overhang; reduce ae; increase spindle RPM |
| Workpiece work hardening | Low feed rate on stainless/titanium | Increase feed to maintain chip thickness > 0.05 mm |
Using the Cutting Speed Calculator
Our free Cutting Speed Calculator lets you enter the recommended surface speed (m/min or SFM) and tool/workpiece diameter to instantly calculate the correct RPM. You can also calculate milling table feed rate from chip load and number of flutes.
Start with the recommended values from the tables above, run a test cut, measure tool wear after 15 minutes, and adjust up or down by 10% increments until you find your optimal working speed.