Correct speeds and feeds are fundamental to CNC machining. Too slow wastes time and causes rubbing. Too fast burns tools and creates poor finishes. This guide covers the formulas, factors, and practical adjustments for optimizing your cuts.
The Core Formulas
Spindle Speed (RPM)
RPM = (SFM × 12) / (π × D)
Simplified: RPM = (SFM × 3.82) / D
Where SFM is surface feet per minute and D is cutter diameter in inches.
Feed Rate (IPM)
Feed = RPM × Chip Load × Number of Flutes
Or: IPM = RPM × FPT × Z
Where FPT is feed per tooth and Z is number of flutes.
Calculate Speeds and Feeds Instantly
Enter material, tool diameter, and number of flutes. Get recommended RPM, feed rate, and chip load.
Surface Speed Guidelines
SFM depends on material and tool:
| Material | HSS (SFM) | Carbide (SFM) |
|---|---|---|
| Aluminum | 300-600 | 800-1500 |
| Mild Steel | 70-100 | 300-500 |
| Stainless 304 | 40-60 | 150-250 |
| Tool Steel | 40-60 | 100-200 |
| Cast Iron | 60-80 | 200-400 |
| Titanium | 30-50 | 100-200 |
Chip Load Basics
Chip load (FPT) is the thickness of material each tooth removes per revolution. Target values for carbide end mills:
| Cutter Dia. | Aluminum | Steel |
|---|---|---|
| 1/8" | 0.001-0.002" | 0.0005-0.001" |
| 1/4" | 0.002-0.004" | 0.001-0.002" |
| 1/2" | 0.004-0.008" | 0.002-0.004" |
| 3/4" | 0.005-0.010" | 0.003-0.005" |
| 1" | 0.006-0.012" | 0.004-0.006" |
Example Calculation
Cutting aluminum with a 1/2" 3-flute carbide end mill at 1000 SFM with 0.005" chip load:
RPM = (1000 × 3.82) / 0.5 = 7640 RPM
Feed = 7640 × 0.005 × 3 = 115 IPM
Adjusting for Conditions
Reduce Speed/Feed When:
- Poor chip evacuation (deep pockets, small tools)
- Long tool stickout causing chatter
- Work hardening materials (stainless, inconel)
- Interrupted cuts
- Older or less rigid machines
Increase Speed When:
- Excellent coolant delivery
- Rigid setup with short stickout
- New, sharp tooling
- Light radial engagement (high-speed machining)
Radial Engagement Effects
Chip thinning occurs with light radial engagement. When step-over is less than 50% of cutter diameter, increase chip load to compensate:
- 50% engagement: Use calculated chip load
- 25% engagement: Increase chip load ~20%
- 10% engagement: Increase chip load ~40%
This is why high-speed machining uses light cuts at high feeds.
Common Mistakes
- Too slow: Creates heat, rubbing, work hardening, poor life
- Wrong chip load: Too low causes rubbing; too high causes breakage
- Ignoring machine limits: Calculate what you need, then limit to machine capability
- Same parameters for all operations: Roughing and finishing need different approaches
Tool Manufacturer Data
Always check the tooling manufacturer's recommendations:
- Specific to their coating and geometry
- Often more aggressive than generic values
- Include depth of cut and step-over guidelines
Start at 70-80% of their recommendations, then optimize based on results.
Speeds and feeds are a starting point, not absolute rules. Listen to the cut—smooth sounds mean good parameters. Chatter, squealing, or excessive heat mean something needs adjustment.
