Skip to content
EN ▾
Feeds & Speeds•5 min read

Feed Rate Formula: RPM, Chip Load and Flutes Explained

A deep dive into the core CNC feed rate formula. Understand the physical relationship between spindle speed, cutting edges, and tooth advance.

By Feed Rate Calculator•Published on March 10, 2026

Worked numbers illustrate arithmetic, not recommended settings for a particular tool or material. Use the tool supplier’s data for your exact application.

The relationship governing table advancement in CNC milling is one of the most elegant and fundamental equations in manufacturing engineering:

F=RPM×Z×fzF = \text{RPM} \times Z \times f_z

At first glance, this is a simple linear multiplication. However, understanding the physical mechanics represented by each variable is what separates novice button-pushers from master CNC machinists.


1. Spindle Speed (RPM): The Frequency of Cut

RPM=RotationsMinute\text{RPM} = \frac{\text{Rotations}}{\text{Minute}}

Spindle RPM dictates the frequency at which cutting edges pass through the workpiece. Every full 360∘360^\circ rotation of the tool brings each of its cutting lips into contact with the shear zone.

RPM is not picked arbitrarily; it is derived from the peripheral cutting speed (VcV_c in m/min or SFM in ft/min) suitable for the tool-workpiece interface:

RPM=1,000×Vcπ×D\text{RPM} = \frac{1,000 \times V_c}{\pi \times D}

If you double your RPM while maintaining the same linear feed rate, each tooth cuts half as much material (fzf_z is halved). Conversely, if you increase RPM while keeping chip load constant, the machine must travel proportionally faster to maintain tooth engagement thickness.


2. Number of Flutes (ZZ): Cutting Density

Z=Cutting EdgesZ = \text{Cutting Edges}

The number of flutes on an end mill determines how many individual chips are cut during each complete revolution:

  • A 2-flute end mill takes 2 cuts per revolution.
  • A 4-flute end mill takes 4 cuts per revolution.
  • A 6-flute end mill takes 6 cuts per revolution.

Because feed rate is total linear velocity per minute, multiplying by ZZ means that more flutes allow higher table feed rates at the exact same RPM and chip load.

Flute CountPrimary ApplicationChip Pocket ClearanceFeed Rate Multiplier
1 - 2 FlutesAluminum, Plastics, WoodMassive chip gullets; prevents chip clogging1.0×1.0\times baseline
3 FlutesHigh-speed Aluminum, SlottingBalanced core strength and chip clearance1.5×1.5\times vs 2-flute
4 FlutesSteels, Stainless, TitaniumStiff core; excellent for finishing and profile milling2.0×2.0\times vs 2-flute
5 - 7 FlutesTrochoidal Dynamic Milling, Hardened SteelsMaximum core rigidity; high table feeds on light stepovers2.5×−3.5×2.5\times - 3.5\times

3. Chip Load (fzf_z): Physical Chip Thickness

fz=Material Thickness per Tooth (mm/tooth or in/tooth)f_z = \text{Material Thickness per Tooth (mm/tooth or in/tooth)}

Chip load is the physical thickness of the slice sheared away by the cutter’s edge.

Why Chip Load Must Never Be Too Low

Cutting edge preparation and material behavior affect minimum chip thickness. Too little feed for the application can increase rubbing rather than clean chip formation. There is no single edge-radius or temperature threshold for all tools.

  • Friction skyrockets
  • Rubbing can generate unwanted heat and wear.
  • Work-hardening occurs on austenitic stainless steels and superalloys
  • The carbide edge micro-chips and wears out rapidly

Why Chip Load Must Not Be Too High

Increasing chip load generally increases cutting force. The relationship depends on material, geometry and engagement; a simple proportional model is not an exponential law. Excessive load can cause:

  • Bending deflection of the cutter (y∝F⋅L33EIy \propto \frac{F \cdot L^3}{3EI})
  • Excessive tool chatter and vibration marks on workpiece walls
  • Chipped flute corners or catastrophic tool snap

Solving the Formula in Reverse

Machinists frequently encounter existing CNC G-code programs where the programmer wrote: S6000 M03 G01 X100. F1200.

To know whether this cut is safe, you must solve in reverse for chip load:

fz=FRPM×Z=1,2006,000×4=0.05 mm/toothf_z = \frac{F}{\text{RPM} \times Z} = \frac{1,200}{6,000 \times 4} = 0.05\text{ mm/tooth}

Use our Chip Load Calculator to instantly analyze existing feed rates and verify cutting parameters.

Formula reference

See Sandvik Coromant’s milling formulas and definitions for the standard relationships between spindle speed, feed per tooth, table feed and cutting volume.

Ready to Calculate Your Feeds and Speeds?

Use our interactive Feed Rate Calculator with formula breakdowns, chip thinning, and MRR.

Open Calculator →
Machining toolkit

Related CNC Machining Calculators

Cutting formulas, spindle speed and material removal calculations