If you are new to CNC milling, one of the first things you will encounter is feeds and speeds.
You may see settings such as:
- 10,000 RPM spindle speed
- 500 mm/min feed rate
- 0.05 mm chip load
- 2 mm depth of cut
- 40% stepover
At first, these numbers can seem arbitrary.
They aren’t.
Feeds and speeds are the cutting conditions used to control how a cutting tool interacts with the material. Choosing them correctly can improve tool life, surface finish, machining time and part quality. Choosing them poorly can cause excessive tool wear, broken cutters, vibration, poor finishes or even damage to the machine or workpiece.
The good news is that the basic concepts are straightforward once you understand what each number represents.
This guide explains spindle speed, feed rate, chip load, depth of cut, stepover and the basic calculations used to determine them.
What Are CNC Feeds and Speeds?
The phrase feeds and speeds generally refers to the cutting parameters used during a machining operation.
The two most important starting points are:
Speed — how fast the cutting tool rotates.
Feed — how quickly the cutting tool moves through the material.
There are several other important parameters, including:
- Chip load
- Depth of cut
- Width of cut
- Stepover
- Plunge rate
- Cutting direction
All of these work together.
Changing one parameter can affect the others.
For example, changing from a 6 mm end mill to a 3 mm end mill changes the appropriate spindle speed. Changing the number of flutes changes the relationship between chip load and feed rate.
The goal is not simply to make the spindle spin as fast as possible or make the machine move as quickly as possible.
The goal is to create appropriate cutting conditions for the particular tool, material and machining operation.
Spindle Speed: RPM
The spindle speed is normally expressed in RPM, which means revolutions per minute.
If a CNC spindle is running at:
10,000 RPM
the cutting tool is rotating 10,000 times every minute.
Spindle speed affects the speed at which the cutting edges of the tool move through the material.
The appropriate RPM depends on factors such as:
- Tool diameter
- Tool material
- Workpiece material
- Cutting operation
- Machine capability
- Tool manufacturer’s recommendations
A small cutter generally needs a higher RPM than a large cutter when similar cutting conditions are being used.
This is because the outer edge of a larger cutter travels farther during each revolution.
Surface Speed
To understand spindle speed more deeply, it helps to understand surface speed.
Surface speed describes how quickly the cutting edge travels around the circumference of the tool.
It is commonly expressed as:
- m/min in metric machining
- SFM (surface feet per minute) in imperial machining
For metric calculations, spindle speed can be estimated using:
RPM = (Cutting Speed × 1000) ÷ (π × Tool Diameter)
Where:
- Cutting Speed is in m/min
- Tool Diameter is in mm
- RPM is revolutions per minute
For example, suppose a tool manufacturer recommends a cutting speed of 100 m/min for a particular application and you are using a 10 mm cutter.
The calculation is approximately:
RPM = (100 × 1000) ÷ (π × 10)
RPM ≈ 3,183
So a starting spindle speed might be around 3,200 RPM, assuming the machine, tool and material are suitable for those conditions.
In real-world machining, you would normally start with the tool manufacturer’s recommended cutting data rather than calculating everything from scratch.
Feed Rate
The feed rate is how quickly the cutting tool moves through the material.
It is commonly expressed in:
mm/min
or:
in/min (IPM)
For example:
Feed rate = 600 mm/min
means the tool is programmed to move through its toolpath at 600 millimetres per minute.
Feed rate is extremely important because it determines how much material each cutting edge removes as the tool rotates.
This brings us to one of the most useful concepts in CNC machining:
chip load.
What Is Chip Load?
Chip load is the approximate thickness of material removed by each cutting edge during one revolution.
It is often expressed in:
mm/tooth
or:
in/tooth
You may also hear it called feed per tooth or Fz.
For example, if a cutter has a chip load of:
0.05 mm/tooth
each cutting edge is intended to remove approximately 0.05 mm of material per revolution under the specified cutting conditions.
Chip load is important because the cutting edge needs to produce a chip.
If the chip is too small, the tool may rub against the material instead of cutting efficiently.
If the chip is too large, the cutting forces can become excessive.
The Feed Rate Formula
One of the most useful CNC formulas is:
Feed Rate = RPM × Number of Flutes × Chip Load
Or:
F = N × Z × Fz
Where:
- F = feed rate
- N = spindle speed in RPM
- Z = number of flutes
- Fz = chip load per tooth
Let’s look at an example.
Suppose you have:
- 10,000 RPM
- 2-flute end mill
- 0.04 mm/tooth chip load
The calculation is:
10,000 × 2 × 0.04 = 800 mm/min
So the calculated feed rate is:
800 mm/min
This relationship is extremely useful because it shows why you cannot choose a feed rate independently of spindle speed, tool geometry and chip load.
Why Flute Count Matters
The number of flutes on an end mill affects the feed calculation.
Consider two tools:
Tool A: 2 flutes
Tool B: 4 flutes
If both are running at 10,000 RPM with a chip load of 0.04 mm/tooth:
2-Flute Tool
10,000 × 2 × 0.04
= 800 mm/min
4-Flute Tool
10,000 × 4 × 0.04
= 1,600 mm/min
The four-flute tool has twice as many cutting edges, so the theoretical feed rate is twice as high at the same RPM and chip load.
However, this does not mean a four-flute cutter is always better.
Flute count affects chip evacuation, tool strength, available flute space and the suitability of the cutter for different materials and operations.
For example, aluminium machining often benefits from tooling designed with good chip evacuation, while other applications may favor higher flute counts.
Always follow the recommendations for the specific tool.
Chip Evacuation
One reason chip load matters so much is that the chips need somewhere to go.
As the cutting tool removes material, the chips need to leave the cutting zone.
If chips become trapped around the cutter, several problems can occur.
These can include:
- Recutting chips
- Increased heat
- Poor surface finish
- Tool wear
- Tool breakage
This is particularly important when machining materials that produce long or sticky chips.
Coolant, flood coolant, mist or compressed air may be used depending on the machine, material and tooling.
The appropriate chip-management method depends heavily on the application.
Depth of Cut
Feeds and speeds aren’t just about RPM and feed rate.
Another important parameter is depth of cut.
Depth of cut describes how deeply the cutter engages the material.
There are two dimensions worth understanding.
Axial Depth of Cut
This is the depth of the cut along the tool’s axis.
It is sometimes called:
Axial depth of cut (Ap)
For a vertical milling machine, this is commonly associated with how deeply the tool cuts down into the material.
Radial Width of Cut
This describes how much of the tool’s diameter is engaged sideways.
It is sometimes called:
Radial depth of cut (Ae)
For example, if you are using a 10 mm end mill and only 2 mm of the cutter’s diameter is engaged with the material, the radial engagement is 2 mm.
Stepover
Stepover is the distance between adjacent toolpath passes.
It is particularly important during pocketing and 3D machining.
Imagine a 10 mm cutter moving across a flat surface.
If the tool moves over by 5 mm between passes, the stepover is:
5 mm
That’s 50% of the tool diameter.
A smaller stepover means more passes and therefore a longer machining time, but it can produce a different surface finish and cutting condition.
A larger stepover removes material more aggressively but increases tool engagement.
The appropriate stepover depends on the tool, material, operation and desired result.
Roughing vs Finishing
Feeds and speeds often change depending on whether you are roughing or finishing.
Roughing
The purpose of roughing is to remove a large amount of material efficiently.
A roughing operation may use:
- Larger material engagement
- Aggressive material removal
- A larger tool
- Toolpaths designed to maintain relatively consistent cutting conditions
The goal is generally to remove material quickly while keeping cutting forces within acceptable limits.
Finishing
Finishing operations remove the remaining material needed to achieve the final dimensions and surface.
A finishing operation may use:
- Smaller radial engagement
- Smaller stepover
- Different feed rates
- A dedicated finishing tool
- Toolpaths designed specifically for surface quality
Roughing and finishing are therefore different jobs, and they don’t necessarily use the same feeds and speeds.
Conventional Milling vs Climb Milling
Another important concept is the direction in which the cutter moves relative to the material.
The two common terms are:
Climb milling
and
Conventional milling
In climb milling, the cutter moves in the same general direction as the cutting edge’s instantaneous motion at the point of contact.
In conventional milling, the cutter moves in the opposite direction.
On modern CNC machines with suitable rigidity and backlash control, climb milling is commonly used for many operations because it can provide favorable cutting conditions and surface finish.
However, the correct strategy depends on the machine, workholding, material, tool and operation.
This is one area where CNC beginners should follow the recommendations for their particular machine rather than assuming one strategy is universally appropriate.
What Happens If Your Feed Rate Is Too Low?
It might seem logical that a slower feed rate would always be safer.
That’s not necessarily true.
If the spindle is rotating quickly but the feed rate is too low, the cutting edge may take an extremely small chip.
Instead of cutting efficiently, the tool can begin to rub.
This can produce:
- Excessive heat
- Poor tool life
- Poor surface finish
- Material buildup on the cutter
- Unwanted work hardening in some materials
The exact symptoms depend on the material and tooling.
A cutter that is rubbing is not necessarily being treated gently.
What Happens If Your Feed Rate Is Too High?
If the feed rate is too high for the selected spindle speed, tool and cutting conditions, chip load can become excessive.
Possible results include:
- High cutting forces
- Chatter
- Poor surface finish
- Tool deflection
- Tool breakage
- Machine overload
This is why increasing feed rate should not be done blindly.
The machine, tool and workholding all have physical limits.
What Happens If RPM Is Too High?
Running a cutter too fast can increase heat and cutting-edge wear.
Depending on the material and tool, excessive RPM may cause:
- Rapid tool wear
- Excessive heat
- Poor surface finish
- Material buildup
- Premature tool failure
Small-diameter tools often require higher RPM than large tools to achieve a comparable surface speed, but every tool has a practical limit.
The maximum spindle speed of the machine and the maximum recommended RPM of the tool or holder must also be respected.
What Happens If RPM Is Too Low?
Running too slowly can also be problematic.
If the cutting conditions are not appropriate, the tool may generate excessive cutting forces or produce poor surface finish.
A common mistake is to assume:
“Slower is always safer.”
Instead, think of feeds and speeds as a balanced system.
The spindle speed, feed rate, chip load, tool engagement, material and tooling all need to work together.
Why Tool Diameter Changes Everything
Tool diameter has a major effect on cutting conditions.
Suppose you have:
- A 3 mm end mill
- A 12 mm end mill
They cannot generally be treated as though they were the same tool.
The 12 mm cutter has a much larger circumference and therefore travels much farther per revolution at the same RPM.
The smaller tool also has less physical strength and may require different cutting conditions.
This is why tool manufacturers normally provide cutting data based on specific tool geometries and sizes.
A Practical Feeds and Speeds Example
Let’s work through a simplified example.
Suppose you are using a:
- 6 mm diameter
- 2-flute carbide end mill
- 8,000 RPM spindle speed
- 0.03 mm/tooth chip load
The feed calculation is:
Feed = RPM × Flutes × Chip Load
Feed = 8,000 × 2 × 0.03
Feed = 480 mm/min
So the starting feed rate would be:
480 mm/min
Now imagine you increase the spindle speed to 12,000 RPM while keeping everything else unchanged.
The new theoretical feed rate becomes:
12,000 × 2 × 0.03 = 720 mm/min
This demonstrates an important relationship:
If spindle speed changes and you want to maintain the same chip load, feed rate needs to change as well.
Start With Manufacturer Data
For beginners, one of the best sources of cutting information is the tool manufacturer.
Many manufacturers publish recommended cutting parameters for their tools.
These may include:
- Recommended surface speed
- Chip load
- Maximum RPM
- Feed rate
- Axial depth of cut
- Radial engagement
- Material-specific recommendations
This information is generally a better starting point than copying random feeds and speeds from an internet forum.
Two tools that look almost identical can have very different recommended cutting conditions because of differences in:
- Carbide grade
- Coating
- Geometry
- Helix angle
- Number of flutes
- Edge preparation
- Intended application
Use published data where possible, then adjust carefully based on your machine and actual cutting conditions.
Machine Rigidity Matters
A feeds-and-speeds chart does not know everything about your setup.
A large industrial machining center with a rigid fixture can handle cutting conditions that might be completely unsuitable for a small desktop CNC.
The same tool and material may require different parameters depending on:
- Machine rigidity
- Spindle power
- Tool stickout
- Workholding
- Part geometry
- Material thickness
- Machine condition
This is why manufacturer cutting data should be treated as a starting point rather than an unconditional guarantee.
Tool Stickout Matters Too
Tool stickout is the amount of tool extending from the holder.
Longer stickout increases the tool’s tendency to deflect and vibrate.
As a general principle:
Keep tool stickout as short as practical for the operation.
A short, rigid tool setup can usually tolerate more aggressive cutting than a long, flexible setup using the same cutter.
This is particularly important with small-diameter end mills.
Understanding Chatter
One of the most recognizable CNC machining problems is chatter.
Chatter is unwanted vibration during cutting.
You may hear it as a loud, distinctive buzzing or rattling sound.
It can produce:
- Poor surface finish
- Visible marks on the part
- Tool wear
- Tool breakage
- Excessive machine vibration
Chatter can have many causes, including:
- Excessive tool stickout
- Weak workholding
- Insufficient machine rigidity
- Incorrect cutting parameters
- Tool deflection
- Resonance
Don’t assume that changing RPM alone will always solve chatter.
The entire machining setup needs to be considered.
Feeds and Speeds Are Not Universal Numbers
One of the biggest mistakes beginners make is searching for a single “correct” feeds and speeds setting.
There isn’t one universal setting.
For example, the correct settings for a 6 mm carbide end mill cutting aluminium on one machine may not be appropriate for:
- The same tool cutting steel
- A different machine
- A different toolpath
- A different depth of cut
- A different tool stickout
- A different grade of carbide
- A different aluminium alloy
Instead of memorizing numbers, learn the relationships.
Think about:
Tool → Material → RPM → Chip Load → Feed → Engagement → Machine
These variables form a system.
A Simple Beginner’s Method
When starting a new CNC milling job, a sensible approach is:
1. Identify the material
Aluminium, mild steel, stainless steel, plastic, wood and other materials require different cutting conditions.
2. Identify the tool
Know the diameter, flute count, material and manufacturer’s recommended data.
3. Check the manufacturer’s cutting data
Use this as your primary starting point.
4. Check your machine
Make sure the machine can achieve the required spindle speed and feed rate and has sufficient rigidity and power.
5. Check your setup
Make sure the tool stickout and workholding are appropriate.
6. Set conservative starting conditions where appropriate
If you’re uncertain, use a sensible starting point within the manufacturer’s recommendations and increase performance gradually after confirming the setup behaves correctly.
7. Watch and listen
During machining, pay attention to:
- Sound
- Vibration
- Chip shape
- Surface finish
- Tool wear
- Machine load
8. Make controlled adjustments
Change one parameter at a time where practical.
This makes it much easier to understand what caused an improvement or problem.
What Do Good Chips Look Like?
The chips produced during machining can tell you a lot about what’s happening at the cutter.
The ideal chip appearance depends heavily on the material and cutting conditions.
As a general principle, you want the tool to be cutting material rather than rubbing against it.
Chip color can also provide clues about heat, particularly when machining metals, but color alone should not be used as a precise diagnostic.
More useful observations include:
- Are chips being evacuated effectively?
- Is the tool producing a consistent cut?
- Is there excessive heat?
- Is material sticking to the cutting edges?
- Is the surface finish changing?
- Is the tool wearing unusually quickly?
With experience, machinists learn to combine these observations with machine sound and cutting performance.
The Most Important Feeds and Speeds Formulas
For beginners, these are the main formulas worth knowing.
Spindle Speed
RPM = (Cutting Speed × 1000) ÷ (π × Tool Diameter)
For metric cutting speed in m/min and tool diameter in mm.
Feed Rate
Feed Rate = RPM × Number of Flutes × Chip Load
Or:
F = N × Z × Fz
Chip Load
Rearranging the feed formula gives:
Chip Load = Feed Rate ÷ (RPM × Number of Flutes)
These formulas aren’t intended to replace manufacturer data.
They help you understand how the numbers relate to one another.
A Quick Feeds and Speeds Checklist
Before pressing Cycle Start, ask:
- What material am I machining?
- What tool am I using?
- What is the tool diameter?
- How many flutes does it have?
- What spindle speed am I using?
- What chip load am I targeting?
- What feed rate does that produce?
- What depth of cut am I taking?
- What stepover am I using?
- How much tool stickout do I have?
- Is the workpiece securely held?
- Can my machine handle the planned cutting conditions?
- Does the tool manufacturer provide recommended cutting data?
- Have I simulated and checked the toolpath?
If you can answer these questions, you have already moved beyond simply guessing at feeds and speeds.
Final Thoughts
Feeds and speeds can seem complicated because there are many variables involved.
But the fundamental idea is simple.
Spindle speed controls how fast the tool rotates.
Feed rate controls how fast the tool moves.
Chip load describes how much material each cutting edge removes.
Depth of cut and stepover describe how much material the tool engages.
And all of these parameters need to work together with the:
Tool + Material + Machine + Workholding + Toolpath
The most important lesson for a beginner is not to memorize a table of numbers.
Instead, learn how the numbers are connected.
Once you understand the relationship between RPM, chip load and feed rate, feeds and speeds become much less mysterious—and you have the foundation needed to start optimizing your CNC milling operations.
