What is Chipload?
Chipload (also called "chip load," "feed per tooth," or "FPT") is the thickness of material each cutting edge removes in one revolution of the spindle.
Think of it this way: as the tool spins and moves through material, each flute takes a "bite." Chipload is the size of that bite.
Each flute takes one bite per revolution
The goal is to produce actual chips, not dust
Why Chipload Matters
Chipload is more important than RPM or feed rate alone because it determines:
- Heat management: Chips carry heat away from the cut. Bigger chips = better cooling.
- Tool life: Proper chipload means cutting, not rubbing. Rubbing = friction = heat = dead tool.
- Cut quality: Correct chipload gives clean edges. Wrong chipload gives burning, fuzz, or chatter.
- Tool survival: Too aggressive chipload breaks tools. Too conservative dulls them from heat.
Key insight: You can run the same chipload at different RPM/feed combinations. 18,000 RPM at 100 ipm produces the same chipload as 12,000 RPM at 67 ipm (for a 2-flute tool). The ratio is what matters.
The Formula
Where:
- Feed Rate = How fast the tool moves horizontally (inches/min or mm/min)
- RPM = Spindle speed (revolutions per minute)
- Flutes = Number of cutting edges on the tool
Example 1: Calculate Chipload
Your settings: 18,000 RPM, 100 ipm feed rate, 2-flute end mill
That's about 2.8 thousandths of an inch per tooth—a reasonable chipload for wood.
You can also rearrange the formula to find feed rate:
Example 2: Calculate Required Feed Rate
You want a chipload of 0.002" with a 2-flute tool at 16,000 RPM
So you'd set your feed rate to approximately 60-65 ipm.
When Chipload is Too Low
If chipload is too low, the tool is rubbing more than cutting. Symptoms:
- Dust instead of chips: You get fine powder, not flakes or curls
- Burning or smoke: Friction generates heat faster than it's removed
- High-pitched whine: The tool screams instead of humming
- Hot tool: Touch (carefully!) after the cut—it shouldn't be hot
- Premature tool wear: Friction destroys the cutting edge
Fix: Increase feed rate or decrease RPM. Most beginners run WAY too slow because they're scared. The irony is that going too slow actually damages tools faster than running proper feeds.
When Chipload is Too High
If chipload is too high, you're overloading the tool. Symptoms:
- Chatter: Vibration, rough surface, visible ridges
- Deflection: Tool bends, cuts come out wrong dimensions
- Broken tools: The ultimate symptom—tool snaps
- Motor strain: Spindle sounds labored, might stall
- Rough edges: Tearout, fuzzy surfaces
Fix: Decrease feed rate or increase RPM. Also consider reducing depth of cut—even correct chipload can overload a tool if you're cutting too deep.
Finding the Sweet Spot
The ideal chipload produces:
- Actual chips: Small curls, flakes, or ribbons—NOT dust
- Clean edges: No burning, no fuzz, no tearout
- Smooth sound: Consistent hum, not screaming or chattering
- Warm (not hot) tool: Some heat is normal, burning hot is not
The sweet spot varies by material, but here's a general target:
Chipload by Material
| Material | Chipload Range | Notes |
|---|---|---|
| Hardwood Oak, Maple, Walnut |
0.001" – 0.003" | Start conservative, sharp tools essential |
| Softwood Pine, Cedar, Poplar |
0.002" – 0.004" | Forgiving, can push harder |
| Plywood Baltic Birch, etc. |
0.001" – 0.003" | Glue layers are hard on tools |
| MDF | 0.002" – 0.005" | Consistent, dusty—need good extraction |
| Acrylic/Plastic | 0.003" – 0.007" | Higher chipload prevents melting |
| HDPE/UHMW | 0.004" – 0.008" | Very high chipload, single flute |
| Aluminum | 0.001" – 0.002" | Conservative, use cutting fluid |
These are starting points for hobby CNCs. Industrial machines with more rigid frames and powerful spindles can run more aggressive chiploads.
How Flute Count Affects Chipload
More flutes = more cuts per revolution = need more feed to maintain chipload.
Same RPM and Feed, Different Flutes
18,000 RPM, 100 ipm feed rate:
- 1 flute: 100 ÷ (18,000 × 1) = 0.0056" chipload
- 2 flute: 100 ÷ (18,000 × 2) = 0.0028" chipload
- 3 flute: 100 ÷ (18,000 × 3) = 0.0019" chipload
Notice how the 3-flute has HALF the chipload of the 1-flute at the same settings. You'd need to double the feed rate to match.
This is why:
- 1-2 flutes are best for plastics, aluminum, and when feed rate is limited
- 3+ flutes require fast feed rates and are better for finishing passes
Common Mistakes
Mistake 1: Focusing on RPM Alone
"My router goes to 24,000 RPM so I should use that, right?"
Wrong. Higher RPM needs higher feed rate to maintain chipload. If you can't feed fast enough, you'll be rubbing, not cutting.
Mistake 2: Going Too Slow "To Be Safe"
"I'll just run slow to be careful."
Counterproductive. Running too slow creates heat and destroys tools faster than running proper speeds. "Safe" is the correct chipload, not the slowest speed.
Mistake 3: Ignoring Flute Count
"I'll just use the same settings for my 1-flute and 3-flute bits."
Wrong. A 3-flute at the same feed as a 1-flute has 1/3 the chipload. Always recalculate when changing tools.
Mistake 4: Using Manufacturer Specs Blindly
"The manufacturer says 80 ipm so that's what I'll use."
Maybe. Manufacturer specs assume industrial machines. Your hobby CNC may need adjustment. Always test.
Using the Calculator
We built a free chipload calculator to make this easy:
- Enter your RPM
- Enter your feed rate
- Select flute count
- Choose your material
The calculator instantly shows your chipload and whether it's in the optimal range for your material.
Go further: The calculator gives you a starting point. Our full testing tool generates actual test G-code and walks you through dialing in parameters based on real cut results—not just math.