Cutting speed is the most important starting value in CNC milling. From it you derive spindle speed and feed rate, and with them you decide whether a tool cuts cleanly, lasts a long time or wears out prematurely. In this guide we show how to calculate cutting speed, which values apply to common materials and how to determine the right spindle speed from the cutting speed.
What is cutting speed?
Cutting speed (denoted in machining by the symbol vc) describes how fast the cutting edge of the tool moves relative to the material. It is measured in metres per minute (m/min). Put visually: if you were to roll a point on the outer edge of the milling cutter along a surface, it would cover vc metres per minute.
Cutting speed is a material property in combination with the cutting material. It depends on which material you are machining and what the tool is made of. It is NOT freely selectable but is specified by the tool manufacturer or from empirical tables. From it you then calculate the spindle speed that you actually set on the spindle.
Calculating Cutting Speed: The Formula
Cutting speed, spindle speed and tool diameter are linked by a single basic formula:
vc = (π × d × n) / 1000
- vc = Cutting speed in m/min
- d = Tool diameter in mm
- n = Spindle speed in rpm (revolutions per minute)
- π = Circle constant, approx. 3.14159
- 1000 = Conversion factor from millimetres to metres
In practice, you know the recommended cutting speed (from the table further down) and your tool diameter; what you are looking for is the spindle speed. To find it, you rearrange the formula:
n = (vc × 1000) / (π × d)
Worked Example
You are milling aluminium with a solid carbide milling cutter of 6 mm diameter. The recommended cutting speed is around 250 m/min. This gives:
n = (250 × 1000) / (3.14159 × 6) = 250,000 / 18.85 ≈ 13,263 rpm
So you would set the spindle speed to about 13,000 rpm. If the value is above the maximum speed of your spindle, you must either choose a larger tool diameter or work with a reduced cutting speed.
Cutting Speed Table by Material
The following guide values apply to solid carbide milling cutters. They are intended as a starting point: the actual values depend on alloy, coating, tool geometry and machine rigidity. Start in the middle range and work your way towards your machine.
| Material | Cutting speed vc (m/min) | Note |
|---|---|---|
| Softwood (spruce, pine) | 300–600 | High spindle speeds, sharp tools |
| Hardwood (beech, oak) | 250–500 | Observe the grain direction |
| MDF / chipboard | 300–500 | High tool wear due to binders |
| Acrylic (PMMA) | 200–500 | Risk of melting: cool, remove chips |
| Hard plastics (POM, PA, PE) | 200–600 | Good chip evacuation required |
| Aluminium (wrought alloys) | 200–600 | Special aluminium cutters, minimum quantity lubrication; significantly more possible on rigid machines |
| Brass | 100–250 | Easy to machine, short chips |
| Mild steel (S235) | 40–120 | Rigid machine and cooling required |
| Stainless steel (V2A) | 50–120 | Low values, high demands on the machine |
For detailed cutting data by material, you will find further tables in our practical guides, for example for aluminium machining, milling wood and plastics machining.
From Cutting Speed to Feed Rate
Tip: The interactive cutting data calculator does both steps at once, and the complete relationship between spindle speed, feed rate and depth of cut is explained in the guide Calculating Spindle Speed and Feed Rate.
With the calculated spindle speed, only half the work is done. Just as important is the feed rate, i.e. how fast the tool moves through the material. It determines the chip thickness per flute and thus tool life, surface finish and cutting force.
The feed rate is calculated from the feed per tooth fz (mm per flute):
vf = fz × z × n
- vf = Feed rate in mm/min
- fz = Feed per tooth in mm per flute
- z = Number of flutes
- n = Spindle speed in rpm
We describe the complete cutting data calculation with feed-per-tooth tables, cutting depths and practical examples in detail in the guide Calculating Spindle Speed and Feed Rate.
Common Mistakes with Cutting Speed
- vc too high with steel: Leads to heat build-up, tool wear and discolouration. It is better to set it lower and work with cooling.
- vc too low with aluminium: The material smears and chips stick to the cutting edge (built-up edge). Aluminium needs high cutting speeds and sharp, polished tools.
- Spindle speed limit ignored: Small tools require high spindle speeds. If your spindle does not deliver enough speed, the effective cutting speed drops, and the surface becomes rough.
- Tool diameter mixed up: The calculation uses the actual cutting circle diameter, not the shank diameter.
The Role of the Spindle
Whether you can actually run the calculated spindle speed depends on your spindle. Small milling cutters for engraving or aluminium often need 20,000 rpm and more. Only HF spindles can do that. Conventional router motors are limited in speed and are better suited to larger tools in wood and plastic.
We explain which spindle suits your requirements in the guide HF Spindle vs. Router Motor. You will find an overview of all available drives in the category Spindles & Router Motors, and the matching tools in the category Milling Tools.
Frequently Asked Questions
How do you calculate cutting speed in milling?
Cutting speed vc is calculated from tool diameter and spindle speed: vc = (π × d × n) / 1000, with d in millimetres and n in revolutions per minute. The result is given in metres per minute. In practice, the cutting speed is specified by the material, and you calculate the spindle speed from it: n = (vc × 1000) / (π × d).
What is the difference between cutting speed and feed rate?
Cutting speed (vc) describes how fast the cutting edge moves relative to the material. It depends on the material and tool and determines the spindle speed. Feed rate (vf) describes how fast the tool moves through the material, measured in millimetres per minute. Both values must be matched to each other: the cutting speed sets the spindle speed, the feed rate the chip thickness per flute.
Which cutting speed for aluminium?
For wrought aluminium alloys, the cutting speed with solid carbide milling cutters is usually between 200 and 600 m/min; on rigid machines, higher values are also possible. Aluminium needs high cutting speeds and sharp, preferably polished tools so that the material does not smear and no built-up edge forms. Good chip evacuation and minimum quantity lubrication improve the result significantly.
Why is the cutting speed so low for steel?
Steel and stainless steel are much harder and tougher than wood, plastic or aluminium. Higher cutting speeds would lead to severe heat build-up at the cutting edge and the tool would wear out quickly. That is why mild steel is machined at around 40 to 120 m/min and stainless steel at only 50 to 120 m/min, in combination with a rigid machine and cooling.
What spindle speed results from the cutting speed?
You calculate the spindle speed with the formula n = (vc × 1000) / (π × d). Example: at a cutting speed of 250 m/min and a 6 mm milling cutter, the result is around 13,000 rpm. The smaller the tool diameter, the higher the spindle speed must be, so small milling cutters often require high-frequency spindles with 20,000 rpm and more.
0 comments