Skip to content

Slide 003: Feeds, Speeds & Chip Load Calculations

Slide Visual

Feeds, Speeds & Chip Load Calculations

Slide Overview

This slide teaches students how to calculate and select appropriate feed rates and spindle speeds for different materials and tools. Understanding chip load is the foundation of productive, safe CNC routing that produces quality results and preserves tool life.

Instruction Notes

The Chip Load Formula

Chip load is the thickness of material each cutting edge removes per revolution:

Chip Load = Feed Rate Γ· (RPM Γ— Number of Flutes)

Or rearranged to find feed rate:

Feed Rate (IPM) = Chip Load Γ— RPM Γ— Number of Flutes

Why Chip Load Matters

Every cutting tool has an optimal chip load range. Cutting outside this range causes problems:

Condition Chip Load Symptoms Consequences
Too Low (rubbing) Below recommended Burning, heat buildup, fine dust instead of chips Tool dulls quickly, burn marks on material, fire risk
Optimal Within range Clean chips, smooth cut, no burning Good finish, long tool life, efficient cutting
Too High (overloaded) Above recommended Rough cut, tool deflection, chattering Tool breakage, poor finish, machine strain
Material ΒΌ" 2-Flute (in/tooth) β…›" 2-Flute (in/tooth) Notes
Softwood (pine, cedar) 0.003–0.005 0.002–0.004 Aggressive OK
Hardwood (oak, maple) 0.003–0.005 0.002–0.003 Reduce for figured grain
Plywood/MDF 0.003–0.005 0.002–0.004 MDF is abrasive β€” dulls tools faster
Acrylic (cast) 0.003–0.006 0.002–0.004 Use single-flute or O-flute
HDPE/Delrin 0.004–0.007 0.003–0.005 Plastics need aggressive chip load
Aluminum (6061) 0.001–0.003 0.001–0.002 Use single-flute, add lubrication
Foam (rigid) 0.010–0.020 0.005–0.010 Very aggressive, high feed rates

Example Calculation

Cutting ΒΎ" plywood with a ΒΌ" 2-flute upcut end mill at 18,000 RPM: - Target chip load: 0.004" per tooth - Feed Rate = 0.004 Γ— 18,000 Γ— 2 = 144 IPM - Stepdown: 50% of tool diameter = 0.125" - Number of passes for ΒΎ" material: 6 passes at 0.125" each

Adjusting Speeds and Feeds

Start conservative and adjust based on results: - Burning/heat: Increase feed rate (first choice) or decrease RPM - Chattering/rough cut: Decrease stepdown, check tool runout, reduce feed rate - Tool deflection: Reduce stepdown and stepover, use shorter tool or larger diameter - Fuzzy edges (wood): Use downcut bit for top surface, increase RPM slightly

Surface Speed (SFM) Reference

SFM = (Ο€ Γ— Tool Diameter Γ— RPM) Γ· 12

For a ΒΌ" bit at 18,000 RPM: SFM = (3.14159 Γ— 0.25 Γ— 18,000) Γ· 12 = 1,178 SFM

Key Talking Points

  1. Chip load is THE critical parameter β€” it determines cut quality and tool life
  2. Too slow is just as bad as too fast β€” rubbing burns the material and dulls the tool
  3. Always calculate before cutting β€” do not guess at feed rates
  4. Start with manufacturer's recommended chip load, then adjust based on results
  5. Different materials require different chip loads even with the same tool

Learning Objectives (Concept Check)

  • [ ] Calculate feed rate from chip load, RPM, and flute count
  • [ ] Identify symptoms of chip load that is too low vs. too high
  • [ ] Select appropriate chip load values for 3 different materials

Last Updated: 2026-03-19