Engineering Reference — Quick Look-Up
The formulas, conversions, and reference tables you need on the shop floor. For automatic calculation, use the Engineering Tools — this page is for understanding the math.
Core Machining Formulas
Spindle Speed from Cutting Speed
RPM = (1000 × vc) / (π × D)
vc = cutting speed (m/min), D = tool diameter (mm)
Imperial: RPM = (12 × SFM) / (π × D)
Feed Rate
vf = fz × z × RPM
vf = feed rate (mm/min), fz = feed per tooth (mm), z = number of flutes
Material Removal Rate (MRR)
Milling: MRR = ap × ae × vf (mm³/min)
Turning: MRR = ap × f × vc (mm³/min, f = feed per rev)
Drilling: MRR = π/4 × D² × vf
Cutting Time
t = L / vf
L = total tool travel length (mm), vf = feed rate (mm/min)
Tool Life (Taylor Equation)
V × Tn = C
V = cutting speed, T = tool life (min), n and C = material constants
Unit Conversions
| From | To | Multiply by |
|---|---|---|
| mm | inches | 0.03937 |
| inches | mm | 25.4 |
| m/min | SFM (ft/min) | 3.281 |
| SFM | m/min | 0.3048 |
| mm/min | IPM (in/min) | 0.03937 |
| IPM | mm/min | 25.4 |
| mm/rev | IPR (in/rev) | 0.03937 |
| N·m | ft·lb | 0.7376 |
| bar | psi | 14.504 |
| °C | °F | (°C × 9/5) + 32 |
Trigonometry Quick Reference
Every machinist needs basic trig for angles, tapers, and bolt circles.
| Function | Formula | Used for |
|---|---|---|
| Sine | sin(θ) = opposite / hypotenuse | Angles, taper, chord calculations |
| Cosine | cos(θ) = adjacent / hypotenuse | Horizontal/vertical components |
| Tangent | tan(θ) = opposite / adjacent | Setover, taper per side |
| Pythagorean | c = √(a² + b²) | Diagonal distances, bolt circle coordinates |
Example: taper angle. A part tapers from 30 mm to 20 mm over 50 mm length. The angle per side is:
tan(θ) = ((30 − 20)/2) / 50 = 5 / 50 = 0.1
θ = arctan(0.1) = 5.71°
Common Metric Tap Drill Sizes
| Thread | Pitch (mm) | Tap drill (mm) | % of thread |
|---|---|---|---|
| M3 | 0.5 | 2.5 | ~75% |
| M4 | 0.7 | 3.3 | ~75% |
| M5 | 0.8 | 4.2 | ~75% |
| M6 | 1.0 | 5.0 | ~75% |
| M8 | 1.25 | 6.8 | ~75% |
| M10 | 1.5 | 8.5 | ~75% |
| M12 | 1.75 | 10.2 | ~75% |
| M16 | 2.0 | 14.0 | ~75% |
Surface Finish Quick Reference
| Ra (µm) | Ra (µin) | Typical process |
|---|---|---|
| 0.2 | 8 | Grinding, honing, polishing |
| 0.4 | 16 | Fine grinding, fine boring |
| 0.8 | 32 | Finish milling/turning |
| 1.6 | 63 | Standard machining |
| 3.2 | 125 | Light milling/turning |
| 6.3 | 250 | Rough machining |
| 12.5 | 500 | Drilling, roughing |
Recommended Starting Speeds by Material (vc, m/min)
| Material | HSS tool | Carbide (uncoated) | Coated carbide |
|---|---|---|---|
| Aluminum | 150–300 | 300–600 | 400–800 |
| Brass/Copper | 60–100 | 150–300 | 200–400 |
| Low carbon steel | 25–40 | 100–150 | 200–300 |
| Alloy steel (hardened) | 15–25 | 60–100 | 120–200 |
| Stainless 304/316 | 20–30 | 80–120 | 150–250 |
| Cast iron | 20–40 | 80–150 | 100–250 |
| Titanium | 20–30 | 50–80 | 80–120 |
| Inconel | 10–20 | 30–50 | 60–100 |
Remember: these are starting values. Adjust based on machine rigidity, tool condition, coolant, and surface finish requirements. See Chapter 02 — Machining Parameters for detailed explanations.