Slide 002: Cutting Theory — Speed, Feed, and Depth of Cut¶
Slide Visual¶
Slide Overview¶
This slide covers the three fundamental machining parameters—cutting speed, feed rate, and depth of cut—and how they interact to determine material removal rate, surface finish, tool life, and safety.
Instruction Notes¶
The Three Parameters¶
Every machining operation is defined by three parameters that the operator must set correctly:
1. Cutting Speed (V) — Surface Feet per Minute (SFM) The linear velocity at which the cutting edge moves relative to the workpiece. Each material has a recommended SFM range based on the cutting tool material.
| Workpiece Material | HSS (SFM) | Carbide (SFM) |
|---|---|---|
| Mild Steel (1018) | 80-100 | 300-500 |
| Medium Steel (4140) | 60-80 | 200-350 |
| Stainless Steel (304) | 40-60 | 150-250 |
| Aluminum (6061) | 200-300 | 800-1500 |
| Brass | 150-250 | 500-800 |
| Cast Iron | 50-80 | 250-400 |
Converting SFM to RPM (Lathe): RPM = (SFM × 3.82) / Workpiece Diameter (inches)
Converting SFM to RPM (Mill): RPM = (SFM × 3.82) / Cutter Diameter (inches)
2. Feed Rate (f) - Lathe: Inches per revolution (IPR). Roughing: 0.005-0.015 IPR. Finishing: 0.002-0.005 IPR. - Mill: Inches per tooth (IPT) × number of teeth × RPM = IPM (inches per minute). Roughing: 0.003-0.008 IPT. Finishing: 0.001-0.003 IPT.
3. Depth of Cut (DOC) The radial depth of material removed per pass. - Roughing: 0.050-0.150" (lathe); 0.050-0.250" (mill, depending on cutter and material) - Finishing: 0.005-0.020" (lathe); 0.010-0.030" (mill)
Material Removal Rate (MRR)¶
MRR = Speed × Feed × Depth of Cut (in appropriate units)
Higher MRR = faster production but more heat, force, and tool wear. The operator balances productivity against surface finish and tool life requirements.
The Speed-Feed-Finish Relationship¶
- Faster speed + lighter feed = better surface finish (finishing parameters)
- Moderate speed + heavier feed + deeper cut = maximum material removal (roughing parameters)
- Excessive speed = rapid tool wear, heat buildup, potential tool failure
- Excessive feed = poor surface finish, increased cutting forces, potential workpiece/tool deflection
- Excessive DOC = machine stalling, tool breakage, workpiece ejection
Chip Formation¶
Proper machining produces chips, not dust. Chip color and shape indicate whether parameters are correct: - Long, curly chips (steel): Good parameters, proper speed and feed - Blue/purple chips: Heat is being carried away in the chip (desirable) - Powdery or dusty: Speed too high or feed too low—rubbing instead of cutting - Very thick, irregular chips: Feed or DOC too aggressive
Key Talking Points¶
- Start conservative—you can always increase speed and feed, but a crashed tool or ejected workpiece cannot be undone
- The SFM table is your starting point—adjust based on machine rigidity, tool condition, and setup
- Chip formation tells you everything about your parameters—learn to read the chips
- Coolant extends the usable range of all three parameters
Learning Objectives (Concept Check)¶
- Can students calculate RPM from SFM and diameter?
- Can students distinguish roughing vs. finishing parameters?
- Do students understand the speed-feed-finish relationship?
Last Updated: 2026-03-19