Feed per Tooth (fz) Explained: The CNC Parameter Behind Feed Rate and Chip Load

This article is part of my CNC & Manufacturing Engineering knowledge base — a growing collection of practical CNC machining guides, engineering tools, and programming resources.

In the previous articles of this CNC Machining Fundamentals series, we discussed two important machining parameters:

• Cutting Speed (Vc) → How fast the cutting edge moves relative to the workpiece surface.
• Spindle Speed (n) → How fast the spindle rotates.

But knowing the correct RPM is only part of the machining process.

Once the spindle starts rotating, we need another answer:

How far should the cutting tool advance while each cutting edge is cutting?

This brings us to one of the most important parameters in CNC milling:

Feed per Tooth — fz

Feed per tooth connects three important machining variables:

• Spindle Speed
• Number of Cutting Teeth
• Feed Rate

Understanding this relationship is much more useful than simply memorizing another formula.

In this article, we will look at:

• What feed per tooth actually means
• Feed per tooth vs. feed rate
• Why the number of cutting edges matters
• How fz is calculated
• How fz determines CNC feed rate
• Practical calculation examples
• Feed per revolution vs. feed per tooth
• The relationship between fz and chip thickness
• Why too much or too little feed can both cause problems
• How tool engagement affects the real cutting condition
• How to select a practical starting fz

Let's begin with the basic idea.

1. What Is Feed per Tooth?

Feed per tooth describes the theoretical distance that the tool advances for each cutting tooth during one spindle revolution.

It is commonly represented by:

fz

and expressed in:

mm/tooth

For example:

fz = 0.05 mm/tooth

means that each cutting tooth is assigned a feed of:

0.05 mm

This is sometimes referred to as chip load per tooth, particularly in practical machining discussions.

However, as we will discuss later, feed per tooth and actual chip thickness are related concepts but should not always be treated as exactly the same thing.

2. Why Feed per Tooth Matters

Imagine a milling cutter rotating at:

2,000 RPM

The spindle speed tells us how fast the tool rotates.

But that alone tells us nothing about how quickly the cutter should travel through the workpiece.

We still need to know:

How much material should each cutting edge attempt to remove?

That is where fz becomes important.

Feed per tooth helps connect the mechanical action of individual cutting edges to the programmed machine feed rate.

Conceptually:

Each tooth takes a cut
↓
Each revolution brings multiple teeth through the cut
↓
The spindle makes many revolutions per minute
↓
The machine advances at a corresponding feed rate

This gives us the basic relationship:

Feed Rate = Feed per Tooth × Number of Teeth × Spindle Speed

or:

Vf = fz × z × n

3. Understanding the Variables

The formula is:

Vf = fz × z × n

Where:

We can rearrange the formula to calculate feed per tooth:

fz = Vf / (z × n)

This is the formula used by the Feed per Tooth function in my CNC Machining Calculator.

But before using the calculator, let's understand what the equation actually means.

4. One Revolution Is Not One Cutting Event

This is an important concept for CNC beginners.

Suppose we have a:

4-flute end mill

During one complete spindle revolution, four cutting edges can pass through the cutting zone.

If:

fz = 0.05 mm/tooth

then the theoretical feed per spindle revolution becomes:

0.05 × 4 = 0.20 mm/rev

Now suppose the spindle rotates at:

2,000 RPM

Then:

0.20 × 2,000 = 400 mm/min

Therefore:

Vf = 400 mm/min

This shows why the number of cutting teeth matters.

The machine is not feeding once per revolution.

Multiple cutting edges can participate during each revolution.

5. Practical Example — Calculating Feed Rate

Suppose we have:

• Spindle Speed = 3,000 RPM
• Number of Teeth = 4
• Feed per Tooth = 0.05 mm/tooth

Using:

Vf = fz × z × n

we get:

Vf = 0.05 × 4 × 3000

Therefore:

Vf = 600 mm/min

The programmed feed rate would therefore be:

600 mm/min

A simplified CNC motion command might look like:

G01 X... F600

Now we can see the complete chain:

fz = 0.05 mm/tooth
    ↓
4 teeth
    ↓
3,000 RPM
    ↓
600 mm/min feed rate

6. Reverse Calculation — Finding Feed per Tooth

Sometimes you already have a CNC program and want to understand what cutting condition it is actually using.

Suppose the program contains:

• Spindle Speed = 2,500 RPM
• Feed Rate = 800 mm/min

and the cutter has:

4 cutting teeth

We can calculate the programmed feed per tooth:

fz = Vf / (z × n)

Therefore:

fz = 800 / (4 × 2500)

fz = 0.08 mm/tooth

This calculation can be very useful when reviewing an existing CNC program.

Instead of simply seeing:

S2500

and:

F800

you can translate those machine commands into a more meaningful cutting parameter:

fz = 0.08 mm/tooth

That makes it easier to compare the program against tooling recommendations or another machining process.

7. Why Number of Teeth Matters

Consider two milling cutters.

Cutter A

• 2 flutes

Cutter B

• 4 flutes

Suppose both use:

n = 3,000 RPM

and:

fz = 0.05 mm/tooth

For Cutter A:

Vf = 0.05 × 2 × 3000 = 300 mm/min

For Cutter B:

Vf = 0.05 × 4 × 3000 = 600 mm/min

Same RPM.
Same feed per tooth.
Different feed rate.

Why?

Because the 4-flute cutter presents twice as many cutting edges per revolution.

This is why copying the feed rate from one tool to another without considering the number of effective cutting teeth can be misleading.

8. What If You Change RPM?

Now suppose we keep:

fz = 0.05 mm/tooth

and:

z = 4

but increase spindle speed from:

3,000 RPM

to:

6,000 RPM

At 3,000 RPM:

Vf = 0.05 × 4 × 3000 = 600 mm/min

At 6,000 RPM:

Vf = 0.05 × 4 × 6000 = 1,200 mm/min

The RPM doubled.

To maintain the same feed per tooth, the feed rate must also double.

This is an extremely important relationship:

If RPM changes, feed rate must also change if you want to maintain the same fz.

This is one reason why changing spindle speed without reviewing feed rate can unintentionally change the cutting condition.

9. RPM and Feed Rate Should Not Be Treated Independently

Imagine a process running at:

• 3,000 RPM
• 600 mm/min
• 4 flutes

The feed per tooth is:

0.05 mm/tooth

Now someone increases the spindle speed to:

6,000 RPM

but leaves the feed rate at:

600 mm/min

The new feed per tooth becomes:

fz = 600 / (4 × 6000)

fz = 0.025 mm/tooth

The RPM doubled, but feed rate stayed the same.

So each cutting edge now receives only half the programmed feed per tooth.

This may be very different from what was originally intended.

That is why CNC parameters should be viewed as connected variables rather than isolated settings.

10. Feed per Tooth vs. Feed per Revolution

These two terms are easy to confuse.

Feed per Tooth — fz

Unit: mm/tooth

This describes feed allocated to each cutting tooth.

It is commonly used in milling calculations.

Feed per Revolution — fn

Unit: mm/rev

This describes how far the tool or workpiece advances during one complete spindle revolution.

This is commonly encountered in turning and drilling.

For a milling cutter with z effective teeth:

Feed per Revolution = fz × z

For example:

• fz = 0.05 mm/tooth
• z = 4

Then:

Feed per Revolution = 0.20 mm/rev

Understanding the difference prevents a very common mistake:

0.05 mm/tooth is not the same as 0.05 mm/rev when multiple cutting edges are involved.

11. Is Feed per Tooth the Same as Chip Thickness?

This is where the subject becomes more interesting.

In everyday machining conversations, fz is often described as:

Chip Load

This is useful as a simplified concept.

But technically, we need to be careful.

The programmed feed per tooth is not always identical to the actual chip thickness produced during milling.

Why?

Because actual chip thickness depends on cutter engagement and geometry.

Factors can include:

• Radial engagement
• Cutter diameter
• Entry and exit angle
• Toolpath
• Cutter geometry
• Milling strategy

So:

fz = programmed feed per tooth

while:

actual chip thickness = result of how the cutting edge engages the material

In many conventional situations, treating fz as a practical chip-load reference works well.

But in more advanced machining, the distinction becomes important.

12. Radial Chip Thinning

One example is:

Radial Chip Thinning

Imagine using a milling cutter with a very small radial engagement.

The cutting edge may not generate a maximum chip thickness equal to the programmed fz.

The actual chip can become thinner.

If this effect is significant, maintaining the desired chip thickness may require adjusting the programmed feed per tooth.

This concept becomes particularly important in:

• Light radial engagement
• High-efficiency milling
• Trochoidal toolpaths
• Certain finishing strategies

This deserves its own dedicated article later.

For now, remember:

Feed per tooth is a programmed parameter. Actual chip thickness depends on how the cutting edge engages the material.

13. Why Not Just Use a Very Small Feed per Tooth?

A common beginner instinct is:

"If I'm worried about breaking the tool, I'll just reduce the feed a lot."

Sometimes reducing feed is appropriate.

But extremely low feed is not automatically safer.

A cutting edge is designed to cut material.

If the chip becomes excessively thin, the edge may spend more time:

• Rubbing
• Sliding
• Generating friction
• Generating heat

rather than forming the intended chip.

This can negatively affect machining performance.

So:

Lower feed does not always mean better tool life.

The cutting edge needs an appropriate chip load to operate effectively.

14. What Happens If Feed per Tooth Is Too High?

On the other side, excessive fz increases the load on each cutting edge.

Possible consequences can include:

• Higher cutting forces
• Excessive tool deflection
• Chatter
• Poor surface finish
• Edge chipping
• Tool breakage
• Excessive spindle load
• Workholding problems

Again, the correct value depends on the complete machining system.

There is no universal fz that works for every tool and material.

15. What Determines the Correct Feed per Tooth?

A practical fz depends on many factors.

Tool Diameter
A small-diameter cutter generally cannot be treated the same as a much larger cutter. Tool stiffness and cutting-edge geometry change with size.

Tool Material
Carbide, HSS, ceramics, and other cutting tool materials have different capabilities.

Workpiece Material
Aluminum, steel, stainless steel, titanium, cast iron, and nickel alloys behave differently during cutting.

Number of Cutting Edges
Flute count influences the relationship between fz and machine feed rate.

Radial Engagement
Small radial engagement can affect actual chip thickness.

Axial Depth of Cut
The amount of cutting-edge engagement influences forces and process behavior.

Tool Overhang
Long overhang reduces rigidity and can increase deflection and vibration risk.

Machine Rigidity
The tool does not cut in isolation. The machine, spindle, holder, fixture, and workpiece form one mechanical system.

Workholding
A rigid fixture and a weak setup cannot always support the same cutting parameters.

Tool Manufacturer Recommendations
Whenever reliable manufacturer data exists for the specific tool and material group, it should be an important starting reference.

16. Why Copying Feed Rate Can Be Misleading

Imagine someone tells you:

"I machine this material at 1,000 mm/min."

That information alone is almost meaningless.

We still need to know:

• What RPM?
• How many teeth?
• What tool diameter?
• What tool?
• What material grade?
• What engagement?

For example:

Process A

• Vf = 1,000 mm/min
• n = 2,500 RPM
• z = 4

Then: fz = 0.10 mm/tooth

Process B

• Vf = 1,000 mm/min
• n = 5,000 RPM
• z = 4

Then: fz = 0.05 mm/tooth

The machine feed rate is identical.

But the feed per tooth is completely different.

This is why experienced machining discussions usually need more context than simply:

"What feed are you running?"

17. Connecting Cutting Speed, RPM and Feed per Tooth

Now we can connect the previous articles.

Suppose:

• Tool Diameter = 10 mm
• Cutting Speed = 120 m/min

First calculate RPM:

n = (1000 × Vc) / (π × D)

n ≈ 3,820 RPM

Now suppose:

• z = 4
• fz = 0.05 mm/tooth

Calculate feed rate:

Vf = fz × z × n

Vf = 0.05 × 4 × 3820

Vf ≈ 764 mm/min

Now we have a complete relationship:

Vc = 120 m/min
    ↓
D = 10 mm
    ↓
n ≈ 3,820 RPM
    ↓
fz = 0.05 mm/tooth
    ↓
z = 4
    ↓
Vf ≈ 764 mm/min

This is the point where separate machining formulas begin to form one connected system.

18. Changing One Parameter Affects Another

This is one of the most important ideas in this entire series.

Machining parameters are connected.

For example:

Increase Cutting Speed
Higher Vc → Higher RPM → Higher feed rate required to maintain the same fz

Increase Number of Teeth
More cutting edges → Higher feed rate required to maintain the same fz

Increase Feed per Tooth
More feed per edge → Higher feed rate → Potentially higher cutting load

The formulas help us understand these relationships.

But the actual machining process determines whether the resulting parameters are appropriate.

19. A Practical Workflow

When establishing a milling process, a simplified parameter workflow might look like this:

Step 1 — Identify the Workpiece Material
Know what you are machining.

Step 2 — Select the Cutting Tool
Consider diameter, tool material, coating, geometry, and number of cutting edges.

Step 3 — Obtain Starting Cutting Data
Use reliable tooling recommendations or validated process knowledge. Identify Vc and fz.

Step 4 — Calculate RPM
n = (1000 × Vc) / (π × D)

Step 5 — Calculate Feed Rate
Vf = fz × z × n

Step 6 — Check the Machine and Setup
Consider maximum RPM, machine power, rigidity, toolholder, tool overhang, fixture, and workpiece stability.

Step 7 — Run and Observe
Look at chip formation, cutting sound, vibration, tool wear, surface finish, and machine load.

Step 8 — Optimize and Validate
Adjust the process based on real machining behavior and validated engineering requirements.

This is much more meaningful than simply entering random RPM and feed values into a CNC program.

20. Engineer's Note

One habit I think is extremely useful when reviewing a CNC program is to stop looking only at:

Sxxxx

and:

Fxxxx

Instead, ask:

What cutting speed does this RPM represent?

and:

What feed per tooth does this feed rate represent?

That changes the way you read a CNC program.

For example:

S3000
F600

does not tell the complete story.

But if we know the cutter is a 4-flute tool, we can calculate:

fz = 0.05 mm/tooth

If we also know the tool diameter, we can calculate the cutting speed.

Now the CNC program begins to describe an actual cutting condition rather than just a collection of machine commands.

That way of thinking becomes especially useful when:

• Troubleshooting a process
• Comparing two programs
• Changing tool diameter
• Changing flute count
• Moving a process to another machine
• Optimizing machining parameters

Understanding the relationship is more valuable than memorizing the number.

21. Use the CNC Machining Calculator

I built a free online CNC Machining Calculator to help with these common calculations.

The current version includes:

• Spindle Speed
• Feed Rate
• Feed per Tooth
• Drilling Parameters
• Cutting Speed
• Material Removal Rate (MRR)

For example, open the Feed per Tooth calculator and enter:

• Feed Rate = 800 mm/min
• Number of Teeth = 4
• Spindle Speed = 2,500 RPM

The result is:

fz = 0.08 mm/tooth

You can then compare this result with the recommended cutting data for your tool and machining application.

22. Common Feed per Tooth Mistakes

Before finishing, here are some common mistakes worth remembering.

Mistake #1 — Copying feed rate without checking RPM.
Same feed rate at different RPM produces different fz.

Mistake #2 — Changing RPM but forgetting to adjust feed rate.
If you want to maintain fz, feed rate must change with RPM.

Mistake #3 — Ignoring flute count.
A 2-flute and 6-flute cutter do not require the same feed rate to maintain the same fz.

Mistake #4 — Assuming lower feed is always safer.
Extremely low chip load can create unfavorable cutting behavior.

Mistake #5 — Treating fz and actual chip thickness as universally identical.
Tool engagement can change the actual chip thickness.

Mistake #6 — Selecting fz without considering the complete setup.
Tooling, material, engagement, rigidity, overhang, and workholding all matter.

23. Final Takeaway

Feed per tooth is much more than another number in a machining formula.

It helps describe how the programmed machine motion relates to the load carried by individual cutting edges.

The fundamental relationship is:

Vf = fz × z × n

or:

fz = Vf / (z × n)

Remember:

• Higher RPM → Higher feed rate required to maintain the same fz
• More cutting teeth → Higher feed rate required to maintain the same fz
• Same feed rate does not mean same cutting condition

And most importantly:

Feed per tooth should be understood together with cutting speed, spindle speed, tool geometry, engagement, and the complete machining system.

What's Next?

We have now built three important pieces of the machining parameter chain:

Cutting Speed — Vc
    ↓
Spindle Speed — n
    ↓
Feed per Tooth — fz

Now we can answer the next question:

How do we turn all of this into the Feed Rate programmed into the CNC machine?

That will be the next article:

CNC Feed Rate Explained: How RPM, Feed per Tooth and Flute Count Work Together

In that article, we will connect:

Vc + D → RPM
RPM + fz + z → Feed Rate

Then we can move one step further into:

Material Removal Rate (MRR)

and start looking at the relationship between machining parameters and productivity.

Free CNC Machining Calculator
👉 https://lilu1626.github.io/cnc-machining-calculator/

About Li Lu | CNC & Manufacturing Engineering

Li Lu is a Machining Development Engineer at GE Vernova Advanced Manufacturing & Repair Technology (AMRT) in Singapore, with 10+ years in CNC machining, process development, and machine tool integration.

• Engineering Knowledge Base: https://lilu1626.github.io/cnc-manufacturing-engineering/
• CNC Machining Calculator: https://lilu1626.github.io/cnc-machining-calculator/
• GitHub: https://github.com/LiLu1626
• LinkedIn: https://www.linkedin.com/in/lu-li-29b464163/