Cutting Speed Explained: What Is Vc and How Do You Select It for CNC Machining?

In my previous article, we discussed how to calculate CNC spindle speed using:

n = (1000 × Vc) / (π × D)

The calculation itself is simple.

But there is one important question that comes before calculating RPM:

Where does the cutting speed — Vc — come from?

If you enter the wrong cutting speed, you can calculate the RPM perfectly and still end up with an unsuitable machining parameter.

That is why understanding cutting speed is more important than simply memorizing the spindle speed formula.

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 this article, we will look at:

• What cutting speed actually means
• Cutting speed vs. spindle speed
• How cutting speed is calculated
• Why diameter matters
• Why different materials require different cutting speeds
• How cutting tool material and coating affect Vc
• Milling vs. turning
• What happens when cutting speed is too high or too low
• How to choose a practical starting cutting speed
• Why manufacturer data and process validation matter

Let's start with the fundamentals.

1. What Is Cutting Speed?

Cutting speed describes the relative surface speed between the cutting edge and the workpiece at the cutting point.

In the metric system, cutting speed is normally expressed as:

Vc = meters per minute (m/min)

In the imperial system, you will commonly see:

SFM = Surface Feet per Minute

Cutting speed is sometimes also called:

Surface Speed

This is different from spindle speed.

Spindle speed tells us how many revolutions occur every minute.

Cutting speed tells us how fast the cutting edge is moving across the material surface.

That difference is fundamental.

2. Cutting Speed vs. Spindle Speed

Consider two cutting tools:

• Tool A = Ø10 mm
• Tool B = Ø100 mm

Suppose both tools rotate at:

1,000 RPM

They have exactly the same spindle speed.

But do they have the same cutting speed?

No.

The Ø100 mm tool has a much larger circumference.

During each revolution, a point on its outside diameter travels much farther than a point on the Ø10 mm tool.

Therefore:

Same RPM does not mean same cutting speed.

This is why diameter is part of the relationship between RPM and Vc.

3. Cutting Speed Formula

For metric machining calculations:

Vc = (π × D × n) / 1000

Where:

This is the reverse relationship of the spindle speed formula:

n = (1000 × Vc) / (π × D)

The two equations describe the same physical relationship.

4. Where Does the Formula Come From?

The idea starts with the circumference of a circle:

C = π × D

Imagine a 50 mm diameter cutter.

Its circumference is:

π × 50 ≈ 157.08 mm

That means a point on the outside diameter travels approximately:

157.08 mm per revolution

Now suppose the cutter rotates at:

1,000 RPM

In one minute, that point travels:

157.08 × 1,000

which equals:

157,080 mm/min

Convert millimeters into meters:

157,080 / 1000 = 157.08 m/min

Therefore:

Vc ≈ 157 m/min

And that gives us:

Vc = (π × D × n) / 1000

The formula is simply describing how far the cutting surface travels every minute.

5. Practical Example

Let's calculate the cutting speed for:

• Tool Diameter = 20 mm
• Spindle Speed = 2,000 RPM

Using:

Vc = (π × D × n) / 1000

we get:

Vc = (π × 20 × 2000) / 1000

Therefore:

Vc ≈ 125.7 m/min

So the cutting speed is approximately:

126 m/min

You can also calculate this using my free CNC Machining Calculator. Select the Cutting Speed calculator and enter:

• Diameter = 20 mm
• Spindle Speed = 2000 RPM

The result will be approximately:

125.66 m/min

6. Why Is Cutting Speed So Important?

Cutting speed directly influences what is happening at the cutting edge.

During metal cutting, the tool is:

• Shearing material
• Generating heat
• Experiencing friction
• Carrying mechanical load
• Producing and evacuating chips

Changing cutting speed changes the conditions at the cutting zone.

That can influence:

• Tool life
• Cutting temperature
• Tool wear
• Surface finish
• Productivity
• Process stability

This is why Vc should not be treated as just another number in a CNC program.

7. Why Different Materials Use Different Cutting Speeds

Now we arrive at one of the most important parts.

Why can't we simply use:

Vc = 200 m/min

for every material?

Because materials behave differently during machining.

Consider:

• Aluminum
• Mild steel
• Stainless steel
• Cast iron
• Titanium alloys
• Nickel-based superalloys

They have different combinations of:

• Hardness
• Strength
• Thermal properties
• Work-hardening behavior
• Abrasiveness
• Chip formation characteristics

As a result, the same cutting speed is not suitable for every material.

For example, many aluminum machining applications can use relatively high cutting speeds.

Heat-resistant alloys may require much more conservative cutting conditions.

But there is an important warning here:

Do not select cutting speed based only on the material name.

"Stainless steel" alone is not enough information.

Neither is "aluminum."

The complete machining condition matters.

8. Tool Material Changes the Cutting Speed

Now imagine machining exactly the same workpiece material using:

• HSS Tool
• Carbide Tool

Should they automatically use the same cutting speed?

No.

Cutting tool materials have different:

• Hot hardness
• Wear resistance
• Toughness
• Thermal behavior
• Strength

A cutting speed appropriate for one tool material may be inappropriate for another.

This is one reason why searching:

"What cutting speed should I use for steel?"

is not specific enough.

A better question is:

"What cutting speed should I use for this material, with this cutting tool, in this operation?"

That is much closer to how machining parameters should actually be selected.

9. Tool Coating Also Matters

Even when two tools are both carbide, they may not perform the same way.

For example, cutting tools may use different:

• Coatings
• Substrates
• Edge preparations
• Geometries
• Grades

These differences can significantly change the recommended cutting conditions.

That is why cutting tool manufacturers normally provide specific machining recommendations for their own products.

When reliable manufacturer data is available, it should usually be one of your primary references when establishing a new machining process.

10. Milling and Turning Use the Same Principle

The cutting-speed relationship applies to both milling and turning:

Vc = (π × D × n) / 1000

But the meaning of D changes.

Milling

For milling, D generally relates to the effective cutting diameter of the rotating tool.

For example:

Ø20 mm End Mill

The relevant diameter is related to the cutter.

Turning

For turning, the workpiece rotates.

Therefore, D relates to the workpiece diameter at the cutting location.

This difference becomes very important when the turning diameter changes.

11. Cutting Speed in Turning

Suppose we are turning a workpiece at:

1,000 RPM

At a diameter of:

100 mm

the cutting speed is:

Vc = (π × 100 × 1000) / 1000

Vc ≈ 314 m/min

Now continue machining until the diameter becomes:

50 mm

while keeping the same:

1,000 RPM

The cutting speed becomes:

Vc ≈ 157 m/min

The RPM has not changed.

But the cutting speed has been reduced by half because the diameter has been reduced by half.

This is why constant surface speed is so useful in CNC turning.

12. Constant Surface Speed — G96

Many CNC lathes provide:

G96 — Constant Surface Speed

Instead of commanding one fixed RPM, the control adjusts spindle speed as the cutting diameter changes.

Conceptually:

Diameter decreases → RPM increases → Vc remains approximately constant

This can help maintain more consistent cutting conditions across changing diameters.

The opposite mode is commonly:

G97 — Constant RPM

With G97, spindle RPM remains fixed unless another spindle command changes it.

Constant surface speed is a very useful subject, but it also introduces important considerations such as maximum spindle speed limits.

I will cover G96 and G97 separately in a future CNC programming article.

13. What Happens If Cutting Speed Is Too High?

It is tempting to think:

Higher cutting speed = faster production = better

But machining does not work that way.

If Vc is too high for the specific tool/material/application combination, possible problems may include:

• Excessive cutting temperature
• Accelerated tool wear
• Reduced tool life
• Edge failure
• Poor surface condition
• Unstable machining

Increasing cutting speed can improve productivity only while the cutting process remains technically and economically acceptable.

There is always a practical operating window.

14. What Happens If Cutting Speed Is Too Low?

Then should we simply use a very low cutting speed to protect the tool?

Again, not necessarily.

An unnecessarily low cutting speed can also create disadvantages:

• Lower productivity
• Longer machining time
• Inefficient machine utilization
• Potentially unfavorable cutting behavior in some applications

The objective is not:

Maximum possible Vc

and it is not:

Minimum possible Vc

The objective is to establish an appropriate cutting condition for the complete machining system.

15. There Is No Universal Cutting Speed

This is one of the most important points in this article.

There is no single cutting speed for:

• Steel
• Stainless Steel
• Aluminum

that is correct for every machining operation.

The practical cutting speed depends on a combination of factors:

• Workpiece Material
• Material Condition / Hardness
• Tool Material
• Tool Grade
• Coating
• Tool Geometry
• Machining Operation
• Cutting Engagement
• Coolant Strategy
• Machine Capability
• Setup Conditions

That is why generic online cutting-speed charts should be treated carefully.

They can help with understanding or provide a rough reference.

But they should not automatically replace application-specific tooling data or validated process knowledge.

16. So How Should I Select Cutting Speed?

For someone learning CNC machining, I recommend thinking about the process in this order.

Step 1 — Identify the Workpiece Material

Be as specific as possible.

Don't stop at:

Steel

if you actually know the material grade and condition.

Step 2 — Identify the Cutting Tool

Determine:

• Tool type
• Tool material
• Insert or cutter grade
• Coating
• Geometry

Step 3 — Identify the Operation

For example:

• Face milling
• Shoulder milling
• Slotting
• Turning
• Facing
• Grooving
• Drilling
• Roughing
• Finishing

Different operations can require different parameter strategies.

Step 4 — Check the Tool Manufacturer's Recommendation

If the manufacturer provides cutting data for your exact tool and material group, this is a strong starting point.

Do not ignore the recommended operating range.

Step 5 — Calculate the Required RPM

Once you have selected an appropriate starting Vc:

n = (1000 × Vc) / (π × D)

Now Vc becomes a machine setting through the RPM calculation.

Step 6 — Check the Machine

Ask:

• Can the spindle reach the calculated RPM?
• Is sufficient power available?
• Is the setup rigid?
• Is the tool overhang reasonable?
• Is the workholding suitable?

Step 7 — Run and Observe

Real machining provides information that the formula cannot.

Observe:

• Tool wear
• Chip formation
• Cutting sound
• Vibration
• Surface finish
• Temperature
• Process stability

Step 8 — Optimize and Validate

If the process is stable, parameters can be optimized within appropriate limits.

The final production parameter should come from a combination of:

Calculation + Manufacturer Data + Machine Capability + Process Observation + Validation

17. Engineer's Note

When I look at machining parameters, I don't like treating Vc, RPM, feed, and depth of cut as completely independent numbers.

They belong to the same machining system.

For example:

• Changing Vc changes RPM.
• Changing RPM changes table feed if feed per tooth is maintained.
• Changing engagement can change cutting forces.
• Changing tool overhang can change stability.

This is why troubleshooting becomes much easier when you understand the relationships between machining parameters rather than simply copying numbers from an existing program.

A good CNC programmer should know the parameter.

A good manufacturing engineer should understand why that parameter is there.

18. Cutting Speed and Spindle Speed Work Together

Let's connect the first two articles in this series.

We now have:

Cutting Speed

Vc = (π × D × n) / 1000

and:

Spindle Speed

n = (1000 × Vc) / (π × D)

So:

Cutting Speed + Diameter → Spindle Speed

And:

Spindle Speed + Diameter → Cutting Speed

These are not two unrelated calculations.

They describe the same physical relationship from two different directions.

19. Try the CNC Machining Calculator

I built a free online CNC Machining Calculator to make these common calculations easier.

The current version includes:

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

For example:

Enter:

• Diameter = 20 mm
• Spindle Speed = 2,000 RPM

into the Cutting Speed calculator.

The result is approximately:

125.66 m/min

The project is part of my ongoing Li Lu | CNC & Manufacturing Engineering platform.

20. Final Takeaway

If you remember only one thing from this article, remember this:

Cutting speed is not simply a number you type into a formula.

It represents the surface speed at the cutting zone and is closely connected to the interaction between:

Tool + Material + Machine + Operation + Cutting Conditions

The formula:

Vc = (π × D × n) / 1000

is easy.

Selecting an appropriate Vc is the engineering part.

Start with reliable cutting-tool data.

Understand the workpiece material.

Understand your tooling.

Check the machine and setup.

Then observe and validate the real machining process.

That is much more valuable than memorizing a table of cutting speeds.

What's Next?

So far, we have connected:

Cutting Speed (Vc) → Spindle Speed (n)

But knowing how fast the tool rotates is still not enough.

The next question is:

How fast should the cutting tool move through the material?

That brings us to:

Feed Rate

And before we can properly understand feed rate, we need to understand another important parameter:

Feed per Tooth — fz

In the next article, I will explain:

Feed per Tooth (fz): What It Means, Why It Matters, and How It Connects RPM to CNC Feed Rate

Then we can connect:

Vc → RPM → Feed per Tooth → Feed Rate

and start seeing machining parameters as one complete system rather than separate formulas.

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

About the Author / 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/