What is the formula for CNC milling table feed rate (vf)?

CNC milling table feed rate is: vf = fz * z * N, where vf is table linear feed speed in mm/min (or inches/min), fz is feed per tooth / chip load (mm/tooth or IPT), z is the number of flutes/teeth on the cutter, and N is spindle speed in RPM.

What is Radial Chip Thinning (RCT) and when does it apply?

When radial width of cut (ae) is less than 50% of cutter diameter (ae < D/2), the maximum chip thickness produced at the tooth entry/exit is significantly smaller than the programmed linear feed per tooth (fz). To maintain the manufacturer recommended chip thickness and avoid tool rubbing/burnishing, the programmed feed must be multiplied by a chip thinning factor: fz_comp = fz_actual / (2 * sqrt((ae/D) - (ae/D)^2)).

How is Material Removal Rate (MRR) calculated for milling?

For CNC milling: MRR = (ap * ae * vf) / 1000 [cm^3/min], where ap is axial depth of cut in mm, ae is radial width of cut in mm, and vf is table feed rate in mm/min. In imperial units: MRR = ap * ae * vf [in^3/min], with ap and ae in inches and vf in inches per minute (IPM).

What is the difference between feed per tooth (fz) and feed per revolution (fn)?

Feed per tooth (fz, also termed chip load) represents the advance of a single cutting edge as it traverses through the workpiece. Feed per revolution (fn) is the total distance the tool advances during one full 360-degree spindle rotation: fn = fz * z. Lathe turning tools have a single active cutting point (z=1), so fn equals fz.

Feed Rate Calculator

Q: How is Material Removal Rate (MRR) calculated for milling?

For CNC milling: MRR = (ap * ae * vf) / 1000 [cm^3/min], where ap is axial depth of cut in mm, ae is radial width of cut in mm, and vf is table feed rate in mm/min. In imperial units: MRR = ap * ae * vf [in^3/min], with ap and ae in inches and vf in inches per minute (IPM).

Q: What is the difference between feed per tooth (fz) and feed per revolution (fn)?

Feed per tooth (fz, also termed chip load) represents the advance of a single cutting edge as it traverses through the workpiece. Feed per revolution (fn) is the total distance the tool advances during one full 360-degree spindle rotation: fn = fz * z. Lathe turning tools have a single active cutting point (z=1), so fn equals fz.

CNC Machining Feed Dynamics & Chip Formation Physics

In metal cutting and CNC machining, feed rate determines the advance velocity of the cutting tool relative to the workpiece. While cutting speed ($V_c$) governs the thermal threshold and rotational surface shearing velocity, the feed rate directly dictates undeformed chip thickness, mechanical cutting forces, tool deflection bending moments, surface scallop crest height, and spindle power consumption.

Programming an incorrect feed rate causes catastrophic machining failures. If the feed rate is programmed too low, chip thickness drops below the micro-honed cutting edge radius ($r_\beta \approx 5 - 20\ \mu\text{m}$), causing the tool to rub and burnish rather than shear. This rubbing generates extreme friction, severe work hardening in austenitic steels and nickel alloys, rapid flank wear, and premature chatter vibration. Conversely, an excessive feed rate overloads tool flutes with chips, packing flutes until the solid carbide shank snaps under extreme torsional shear.

Core Mathematical Equations for Milling Feed Rates

Milling cutters feature multiple discrete teeth or flutes ($z$) distributed symmetrically around the tool circumference. The relationship between individual tooth advance and total table axis velocity is formulated per ISO 13399:

$$v_f = f_z \cdot z \cdot N \quad [\text{mm/min or IPM}]$$

Where:

$v_f$: Linear table feed speed, in millimeters per minute ($\text{mm/min}$) or inches per minute ($\text{IPM}$).
$f_z$: Feed per tooth (chip load), in millimeters per tooth ($\text{mm/tooth}$) or inches per tooth ($\text{IPT}$).
$z$: Total active flute or tooth count on the cutting tool.
$N$: Spindle rotational frequency, in revolutions per minute ($\text{RPM}$).

The total feed distance traversed per one single 360-degree rotation of the spindle is the feed per revolution ($f_n$):

$$f_n = \frac{v_f}{N} = f_z \cdot z \quad [\text{mm/rev or IPR}]$$

Radial Chip Thinning (RCT) & High-Efficiency Milling (HEM)

One of the most vital principles in modern CNC toolpath programming is Radial Chip Thinning. Classical feed rate formulas assume that maximum chip thickness equals the programmed feed per tooth ($h_{\text{max}} = f_z$). However, this assumption is true only when the radial width of cut ($a_e$) equals or exceeds 50% of the cutter diameter ($a_e \ge D/2$).

When executing light radial stepovers typical of High-Efficiency Milling (HEM), trochoidal milling, and dynamic toolpaths ($a_e < 0.25 D$), the tooth enters and exits the workpiece across a narrow circular arc, producing a thin sliver of a chip. The true maximum chip thickness ($h_{\text{ex}}$) is geometrically defined as:

$$h_{\text{ex}} = 2 \cdot f_z \cdot \sqrt{\frac{a_e}{D} - \left(\frac{a_e}{D} \right)^2}$$

If an engineer runs a 12 mm end mill at a 1.2 mm radial stepover ($a_e/D = 0.10$) with a standard catalog chip load of $f_z = 0.05\text{ mm}$, the actual chip thickness produced is only $0.03\text{ mm}$, causing tool rubbing and thermal glaze. To achieve the targeted chip thickness ($h_{\text{target}}$), the programmed feed per tooth must be escalated by the Radial Chip Thinning Factor (RCTF):

$$\text{RCTF} = \frac{1}{2 \cdot \sqrt{\frac{a_e}{D} - \left(\frac{a_e}{D} \right)^2}} \quad \Longleftrightarrow \quad f_{z, \text{programmed}} = f_{z, \text{target}} \cdot \text{RCTF}$$

Radial Engagement Ratio ($a_e / D$)	Radial Chip Thinning Factor (RCTF)	Programmed Feed Multiplier	Effective Machining Benefit
50% (Full Slotting or Heavy Shoulder)	1.00	1.00 × (No compensation)	Standard chip thickness geometry.
30% (Standard Semi-Finishing)	1.09	1.09 × Catalog Feed	Mild thinning compensation.
20% (Typical Roughing Shoulder)	1.25	1.25 × Catalog Feed	25% cycle time reduction.
10% (High-Efficiency Dynamic Milling)	1.67	1.67 × Catalog Feed	67% feed boost with low cutting forces.
5% (High-Speed Trochoidal Peel)	2.29	2.29 × Catalog Feed	129% feed increase without overloading tool.
2% (Finishing Wall Profiling)	3.57	3.57 × Catalog Feed	Prevents microscopic rubbing on finishing walls.

Volumetric Material Removal Rate (MRR)

Material Removal Rate ($\text{MRR}$) quantifies the volume of metal sheared away per unit of machining time. It serves as the primary benchmark for machining efficiency, spindle power sizing, and tooling comparison:

$$\text{MRR} = \frac{a_p \cdot a_e \cdot v_f}{1000} \quad [\text{cm}^3/\text{min}] \quad \Longleftrightarrow \quad \text{MRR} = a_p \cdot a_e \cdot v_f \quad [\text{in}^3/\text{min}]$$

Where $a_p$ is axial depth of cut (mm or in), $a_e$ is radial width of cut (mm or in), and $v_f$ is table feed speed (mm/min or IPM). Spindle net cutting power ($P_c$) is directly proportional to MRR and the specific cutting energy of the workpiece material ($k_c$):

$$P_c = \frac{\text{MRR} \cdot k_c}{60 \times 10^3} \quad [\text{kW}]$$

Where specific cutting force ($k_c$) ranges from 700 $\text{N/mm}^2$ for aluminum up to 2,200 $\text{N/mm}^2$ for alloy steel and 3,200 $\text{N/mm}^2$ for nickel superalloys.

Step-by-Step Worked Case Study: Dynamic Trochoidal Milling in 304 Stainless

Design Scenario: A programmer is setting up a dynamic HEM roughing toolpath on a 5-axis machining center to pocket 304 austenitic stainless steel using a 10 mm 5-flute carbide end mill.

Cutter diameter: $D = 10.0\text{ mm}$, Flutes: $z = 5$.
Spindle speed: $N = 4,200\text{ RPM}$ ($V_c = 132\text{ m/min}$).
Target chip thickness (catalog recommended): $f_{z, \text{target}} = 0.045\text{ mm/tooth}$.
Axial depth of cut: $a_p = 15.0\text{ mm}$ (1.5 × $D$).
Radial width of cut: $a_e = 1.0\text{ mm}$ (10% stepover).

Step 1: Compute Radial Engagement Ratio ($a_e / D$)

$$\frac{a_e}{D} = \frac{1.0}{10.0} = 0.10 \quad (10\%)$$

Step 2: Calculate Radial Chip Thinning Factor (RCTF)

$$\text{RCTF} = \frac{1}{2 \cdot \sqrt{0.10 - (0.10)^2}} = \frac{1}{2 \cdot \sqrt{0.10 - 0.01}} = \frac{1}{2 \cdot \sqrt{0.09}} = \frac{1}{2 \cdot 0.30} = 1.667$$

Step 3: Calculate compensated feed per tooth and linear table feed rate

$$f_{z, \text{comp}} = 0.045 \times 1.667 = 0.075\text{ mm/tooth}$$ $$v_f = f_{z, \text{comp}} \cdot z \cdot N = 0.075 \cdot 5 \cdot 4200 = 1,575\text{ mm/min} \quad (62.0\text{ IPM})$$

Without chip thinning compensation, the feed rate would be only $0.045 \times 5 \times 4200 = 945\text{ mm/min}$. Enabling RCT increases feed speed by 66.7% while keeping true chip thickness at the safe $0.045\text{ mm}$ specification.

Step 4: Compute Volumetric Material Removal Rate (MRR)

$$\text{MRR} = \frac{15.0 \cdot 1.0 \cdot 1575}{1000} = \frac{23625}{1000} = 23.63\text{ cm}^3/\text{min} \quad (1.44\text{ in}^3/\text{min})$$

Frequently Asked Questions

What happens if I enable Radial Chip Thinning on a 50% or full-slot cut?

At 50% radial engagement ($a_e / D = 0.50$), the chip thinning factor mathematically equals 1.00, meaning zero compensation is applied. If engagement exceeds 50% (such as full slotting at 100%), chip thinning does not occur; instead, the chip thickness at entry/exit is already maximized. You should never apply chip thinning multipliers above 50% engagement, as doing so would overload flutes and snap the tool.

Why do 5-flute and 7-flute end mills allow higher feed rates than 3-flute or 4-flute cutters?

Because linear feed rate is directly proportional to flute count ($v_f = f_z \cdot z \cdot N$), a 5-flute end mill delivers a 25% higher table feed than a 4-flute tool at the exact same spindle RPM and chip load. For peripheral dynamic roughing in steel, 5-flute, 6-flute, and 7-flute end mills provide massive productivity gains because the small radial engagement leaves ample open flute space for chip ejection.

How does tool stickout (overhang) constrain allowable feed rates?

Tool deflection is governed by cantilever beam mechanics: deflection $\delta \propto L^3 / D^4$, meaning doubling tool overhang increases deflection by a factor of 8. Excessive deflection causes chatter, poor dimensional tolerances, and chipped cutting corners. When tool overhang exceeds 3 × diameter (e.g., sticking out 50 mm on a 10 mm tool), feed per tooth and axial depth of cut must be reduced by 20% to 50% to prevent chatter resonance.

How do I calculate feed rate for CNC circular interpolation (internal bore milling)?

When an end mill travels along a circular internal bore arc, the tool center line travels along a tighter radius than the outer tool edge touching the wall. The feed rate programmed at the tool center point must be derated by the arc ratio: $v_{f, \text{center}} = v_{f, \text{linear}} \cdot \left(\frac{D_{\text{bore}} - D_{\text{tool}}}{D_{\text{bore}}} \right)$. Conversely, when contouring around an outside boss, the center feed can be increased.

CNC Feed Rate & Material Removal Results