What Are Feeds and Speeds?
"Feeds and speeds" refers to the cutting parameters that determine how your CNC removes material:
- Speed = Spindle RPM (how fast the tool rotates)
- Feed = Feed rate (how fast the tool moves through material)
Getting these right is the difference between clean cuts and burnt wood, broken bits, and chatter. It's the most important skill in CNC work.
The key insight: RPM and feed rate must be balanced. High RPM needs high feed. Low RPM needs low feed. The ratio between them determines chipload—the actual thickness of each chip.
The Key Formula
Everything in feeds and speeds comes down to one formula:
Rearranged to solve for feed rate:
This tells you: given a target chipload and your spindle speed, what feed rate should you run?
Example Calculation
You're cutting hardwood with a 2-flute 1/4" end mill. You want a chipload of 0.002" and your router runs at 18,000 RPM.
Feed Rate = 0.002 × 18,000 × 2 = 72 inches per minute
So you'd set your feed rate to approximately 70-75 ipm.
Spindle Speed (RPM)
RPM is determined by your spindle or router, the tool diameter, and the material. General principles:
- Smaller tools → higher RPM (a 1/8" bit needs more RPM than a 1/2" bit)
- Harder materials → lower RPM (aluminum needs lower RPM than pine)
- Softer materials → higher RPM is OK (but requires matching feed rate)
Typical RPM Ranges
| Tool Diameter | Wood/Plastic | Aluminum |
|---|---|---|
| 1/8" (3mm) | 18,000 - 24,000 | 12,000 - 18,000 |
| 1/4" (6mm) | 16,000 - 20,000 | 10,000 - 16,000 |
| 3/8" (10mm) | 14,000 - 18,000 | 8,000 - 12,000 |
| 1/2" (12mm) | 12,000 - 16,000 | 6,000 - 10,000 |
Router users: Most palm routers (Makita, DeWalt, etc.) have a limited speed range and no digital readout. Use a tachometer or refer to dial charts. Our testing tool includes common router dial settings.
Feed Rate
Feed rate is how fast the tool moves horizontally through material, measured in inches per minute (ipm) or millimeters per minute (mm/min).
Feed rate must be matched to RPM to achieve proper chipload:
- Feed too slow: Tool rubs, generates heat, burns material, wears tool
- Feed too fast: Overloads tool, causes chatter, rough finish, broken bits
Typical Feed Rates for Wood
| Material | Feed Rate Range | Notes |
|---|---|---|
| Softwood (Pine, Cedar) | 80 - 150 ipm | Forgiving, can push faster |
| Hardwood (Oak, Maple) | 60 - 120 ipm | Requires sharp tools |
| Plywood | 60 - 100 ipm | Glue is hard on tools |
| MDF | 80 - 150 ipm | Consistent, dusty |
| Acrylic | 60 - 100 ipm | Higher chipload prevents melting |
| Aluminum | 20 - 60 ipm | Use cutting fluid, clear chips |
Plunge Rate
Plunge rate is how fast the tool moves down into material (Z direction). It should be significantly slower than feed rate—typically 30-50% of horizontal feed.
End mills aren't designed to plunge straight down like drill bits. They cut on the sides, not the tip. Use ramping or helical entry when possible.
Depth of Cut (DOC)
Depth of cut is how deep each pass goes. This is where beginners get into trouble—cutting too deep causes:
- Tool deflection (tool bends, cutting inaccurately)
- Chatter (vibration causing rough surface)
- Broken tools
- Motor strain
General Guidelines
| Material | Max DOC (as % of tool diameter) |
|---|---|
| Softwood | 50 - 100% |
| Hardwood | 25 - 50% |
| Plywood | 50 - 75% |
| MDF | 50 - 100% |
| Plastic | 50 - 100% |
| Aluminum | 10 - 25% |
For a 1/4" tool in hardwood, that means 0.0625" to 0.125" per pass. Yes, it means more passes—but your cuts will be cleaner and your tools will last longer.
Stepover
Stepover is the distance the tool moves over between passes when clearing a pocket or facing a surface. It's usually expressed as a percentage of tool diameter.
- 40-50% stepover: Good balance of speed and finish (most common)
- 60-70% stepover: Faster but rougher finish
- 20-30% stepover: Slower but very smooth finish
For 3D carving with ball nose bits, use smaller stepovers (10-20%) to avoid visible scallops.
Material Guidelines
Softwood (Pine, Cedar, Poplar)
- Very forgiving, good for learning
- Can handle aggressive feeds
- Watch for tearout on end grain
- Upcut bits work well
Hardwood (Oak, Maple, Walnut)
- Requires sharp tools
- More conservative DOC
- Climb milling often gives better finish
- Slower feed, watch for burning
Plywood
- Glue layers are hard on edges
- Use compression bits for clean edges on both faces
- Or downcut for clean top, accept fuzzy bottom
- Feed rate similar to hardwood
MDF
- Very consistent cutting
- Creates LOTS of fine dust—excellent extraction required
- Can run aggressive speeds
- Edges can be fuzzy, seal with CA glue or sanding sealer
Plastics (Acrylic, HDPE)
- Main enemy is HEAT—melts and re-welds
- Use single-flute or O-flute bits
- Higher chipload (bigger chips carry heat away)
- Consider air blast instead of dust collection
- Leave protective film on until done
Aluminum
- Use cutting fluid (WD-40 works for hobby use)
- Single flute or 2-flute with high helix
- Clear chips constantly—recutting chips = heat = problems
- Always ramp or helix into material, never plunge
- Conservative DOC (10-25% of tool diameter)
Troubleshooting
Burning or Smoke
Cause: Chipload too low (rubbing instead of cutting)
Fix: Increase feed rate or decrease RPM
Chatter (Vibration/Rough Surface)
Cause: Tool overloaded, deflection, or resonance
Fix: Reduce DOC, reduce feed rate, or change RPM (sometimes going slightly faster or slower escapes a resonant frequency)
Rough/Fuzzy Edges
Cause: Dull tool, wrong direction, chipload issues
Fix: Try a fresh tool, switch between climb/conventional, adjust chipload
Tool Breaking
Cause: Too aggressive (DOC, feed), chips packing, tool deflection
Fix: Reduce DOC, improve chip clearing, check runout
Melting (Plastics)
Cause: Chipload too low, chips re-welding
Fix: Increase feed rate significantly, use single flute, add air blast
How to Test & Dial In
Theory only gets you so far. Every machine, tool, and material combination is different. The only way to truly dial in your settings is to test.
The Testing Process
- Start with conservative parameters (use our chipload calculator for a baseline)
- Run a test cut on scrap material
- Evaluate: edge quality, chip formation, sound, tool temperature
- Adjust based on results
- Repeat until optimized
Skip the guesswork: Our CNC Manager testing tool automates this process. It generates test G-code, walks you through scoring the cut, and suggests parameter adjustments until you're dialed in.
Signs of a Good Cut
- Clean edges (no tearout or fuzz)
- Chips, not dust (small curls or flakes, not powder)
- Smooth sound (consistent hum, not screaming or chattering)
- Cool tool (warm is OK, hot means problems)