Feed Per Tooth vs Feed Per Revolution in Milling, Lathes, and Drilling

A common source of confusion in CNC machine programming stems from two closely related feed metrics:

• Feed per Tooth ($f_z$): Also known as chip load, measured in $\text{mm/tooth}$ or $\text{IPT}$.
• Feed per Revolution ($f_n$): The linear distance advanced during one full $360^\circ$ rotation of the tool or workpiece, measured in $\text{mm/rev}$ or $\text{IPR}$.

Understanding where and why each metric applies is critical to avoiding broken tooling and improper surface finishes.

---

The Mathematical Connection

In multi-flute milling cutters, feed per revolution is simply the sum of the chip loads taken by all flutes during that single rotation:

$f_n = Z \times f_z$

Where:

• $f_n$ = Feed per revolution ($\text{mm/rev}$ or $\text{IPR}$)
• $Z$ = Number of cutting flutes
• $f_z$ = Feed per tooth ($\text{mm/tooth}$ or $\text{IPT}$)

And consequently:

$\text{Feed Rate } (F) = \text{RPM} \times f_n = \text{RPM} \times (Z \times f_z)$

---

When to Use Which Parameter

1. CNC Milling (End Mills & Face Mills)

In milling, feed per tooth ($f_z$) is the primary engineering design parameter.

• Why? Because each tooth enters and exits the cut intermittently. Tool life and chip formation are dictated by the thickness cut by each individual tooth.
• If you switch an end mill from 2 flutes to 4 flutes while holding $f_z$ constant, $f_n$ doubles, and your linear feed rate doubles.

2. CNC Lathes & Turning (OD Turning, Boring, Parting)

In turning, the workpiece rotates while a stationary single-point insert feeds along the geometry.

• Because there is only one active cutting point engaged continuously, there is no flute distribution.
• Here, feed per revolution ($f_n$ / IPR) is the universal standard.
• Surface finish in turning is directly governed by feed per revolution and the tool nose radius ($r_\epsilon$): $\text{Theoretical Peak-to-Valley Roughness } (R_t) \approx \frac{f_n^2}{8 \times r_\epsilon}$

3. CNC Drilling (Twist Drills & Indexable Drills)

In drilling, cutting tool manufacturers universally specify feed rates in feed per revolution ($f_n$), even though standard twist drills have two cutting lips.

• A $\varnothing 10\text{ mm}$ drill might specify a starting feed of $0.15\text{ mm/rev}$.
• This means the entire drill moves into the hole $0.15\text{ mm}$ per rotation.
• Common Pitfall: Do NOT multiply this drilling catalog feed by 2 flutes! That would double the tool feed and split the drill web or stall the spindle motor.

---

Summary Reference Table

Operation	Standard Specification	Primary Formula	Typical G-Code Mode
Milling	Feed per Tooth ($f_z$)	$F = \text{RPM} \times Z \times f_z$	G94 (Feed per Minute)
Turning	Feed per Revolution ($f_n$)	$F = \text{RPM} \times f_n$	G95 (Feed per Revolution)
Drilling	Feed per Revolution ($f_n$)	$F = \text{RPM} \times f_n$	G95 (Feed per Revolution)

Calculate feeds for all three operations effortlessly using our Feed Rate Calculator or Feed per Revolution Calculator.