The right cutting data are decisive for clean results, long tool life and gentle treatment of your CNC milling machine. In this guide, we explain the formulas and provide a field-tested cutting data table for the most common materials.
The Three Basic Variables
Spindle Speed (n)
The spindle speed is given in revolutions per minute (rpm) and depends on the cutting speed (Vc) and the cutter diameter (d):
n = (Vc × 1000) / (π × d)
Example: Vc = 200 m/min, d = 6 mm → n = (200 × 1000) / (3.14 × 6) = 10,616 rpm
Feed Rate (Vf)
The feed rate determines how fast the tool moves through the material:
Vf = fz × z × n
Where: fz = feed per tooth, z = number of flutes, n = spindle speed
Example: fz = 0.05 mm, z = 2, n = 10,616 → Vf = 0.05 × 2 × 10,616 = 1062 mm/min
Once the feed rate is fixed, you can use it to estimate the run time of a program: Machining Time Calculator.
Depth of Cut (ap and ae)
- ap (axial depth of cut): Cutting depth, i.e. how deep the cutter plunges per pass
- ae (radial depth of cut): Cutting width, i.e. how much material is removed at the side
Rule of thumb: ap at most 1× the cutter diameter, ae at most 50% of the diameter.
ap, ae and feed rate determine the material removal rate, which is how much material your machine removes per minute. Calculate it directly: Material Removal Calculator.
Cutting Data Table by Material
The following values are guideline values for solid carbide end mills (2 flutes, Ø 6 mm) on a CNC gantry milling machine:
| Material | Vc (m/min) | fz (mm) | ap (mm) | ae (mm) | Speed (rpm) | Feed rate (mm/min) |
|---|---|---|---|---|---|---|
| Softwood (spruce, pine) | 300–500 | 0.08–0.15 | 6–12 | 3–4 | 16,000–24,000 | 2500–4000 |
| Hardwood (beech, oak) | 200–350 | 0.05–0.10 | 4–8 | 2–3 | 10,000–18,000 | 1500–2500 |
| MDF / multiplex | 250–400 | 0.06–0.12 | 5–10 | 3–4 | 13,000–21,000 | 2000–3500 |
| Aluminium | 150–250 | 0.03–0.06 | 2–4 | 1–3 | 8,000–13,000 | 500–1500 |
| Plastic (POM, PA) | 200–400 | 0.05–0.10 | 3–6 | 2–4 | 10,000–21,000 | 1500–3000 |
| Acrylic (PMMA) | 100–200 | 0.03–0.06 | 2–4 | 1–3 | 5,000–10,000 | 500–1200 |
| Brass | 100–180 | 0.02–0.05 | 1–3 | 1–2 | 5,000–9,500 | 400–1000 |
The guideline values above apply to solid carbide end mills. You will find suitable milling cutters, drills and sets in the Milling Tools category, and the matching drives under Spindles & Motors.
Common Mistakes in Calculating Cutting Data
- Spindle speed too high for plastic: Leads to melting and material sticking to the cutter
- Feed rate too low: The cutter rubs instead of cutting, which causes heat build-up and faster wear
- Depth of cut too large in aluminium: Overloads the cutter and can cause breakage
- Not adapting cutting data to the spindle: A high-frequency (HF) spindle at 24,000 rpm allows different values than a router motor at 10,000 rpm
Practical Tips
- Always start conservatively and increase gradually
- Listen to the machine: a steady cutting sound indicates optimal parameters
- With aluminium, always use cutting fluid or minimum quantity lubrication
- Document working settings for repeatability
Calculating and Understanding Cutting Speed (vc)
Tip: For quick practical use, there is the interactive Cutting Data Calculator (Spindle Speed & Feed Rate), and a detailed in-depth look in the article Calculating Cutting Speed: Formula & Table.
The cutting speed vc is the speed at which the cutting edge of the cutter travels along the workpiece, given in metres per minute (m/min). It is the central material-dependent variable: every material tolerates only a certain vc range before the cutting edge gets too hot and wear rises sharply. Unlike the spindle speed (rpm), vc is independent of the cutter diameter and can therefore be read directly from tables.
The relationship between cutting speed, spindle speed and cutter diameter is:
vc = (n × π × d) / 1000 [m/min]
Here, n is the spindle speed in rpm, d the cutter diameter in mm and π ≈ 3.1416. In practice, you usually know the desired cutting speed from the table and want to work out the spindle speed from it. To do this, rearrange the formula for n:
n = (vc × 1000) / (π × d) [rpm]
Worked Example: From vc to Spindle Speed
You are milling aluminium with a solid carbide end mill Ø 6 mm and choose vc = 200 m/min from the table:
n = (200 × 1000) / (3.1416 × 6) = 200,000 / 18.85 ≈ 10,610 rpm
With a smaller cutter, the required spindle speed rises considerably. For the same vc value with a Ø 3 mm cutter, n is already approx. 21,200 rpm, a value that can only be reached with a high-speed HF spindle. From the spindle speed determined in this way, you then calculate the feed rate: vf = fz × z × n.
If you do not want to calculate by hand every time, use the interactive cutting data calculator at the top of this page: enter the material, cutter diameter and number of flutes, and the spindle speed and feed rate are calculated automatically from the stored vc and fz values.
Cutting Speed by Material: Focus on Aluminium
The right cutting speed depends primarily on the material. Wood and wood-based materials tolerate very high vc values because they are soft and give hardly any heat back to the cutting edge. Metals such as aluminium and brass are lower because more heat flows into the tool and thermally stresses the cutting edge. The following vc guideline values correspond to the large cutting data table above and apply to solid carbide cutters:
| Material | vc (m/min) | Note |
|---|---|---|
| Softwood (spruce, pine) | 300–500 | Highest values, sharp cutting edges required |
| Hardwood (beech, oak) | 200–350 | Lower feed rate than softwood |
| MDF / multiplex | 250–400 | Highly abrasive, watch tool wear |
| Aluminium | 150–250 | Cooling/MQL and chip evacuation are decisive |
Cutting Speed for Aluminium in Detail
When milling aluminium on a gantry mill, a vc range of 150 to 250 m/min has proved its worth. Within this range, the specific value depends on the alloy, spindle power and chip evacuation:
- Soft wrought alloys (e.g. AlMg, AlMgSi such as EN AW-6060/6082): vc towards the upper end, 200–250 m/min. They machine well but tend to smear; sharp, uncoated or ZrN/DLC-coated cutters with a polished rake face help.
- Cast alloys and hard alloys: vc more like 150–200 m/min, as they are more brittle and harder on tools.
- Number of flutes: usually 1 or 2 flutes in aluminium, so that each cutting edge has enough chip space and the chip is reliably evacuated. Clogged flutes quickly lead to breakage.
Example for a Ø 6 mm cutter, 2 flutes, vc = 200 m/min: n ≈ 10,610 rpm. With fz = 0.04 mm, vf = 0.04 × 2 × 10,610 ≈ 850 mm/min, a conservative, process-reliable starting value that you increase gradually based on sound and chip formation. In aluminium, effective cooling or minimum quantity lubrication is mandatory, otherwise the chip sticks to the cutting edge (built-up edge). You will find further advice on machine and tool selection in the Aluminium Practical Guide; for wood-based materials, take a look at the Wood Practical Guide.
Pro Tip: Chip Thinning Compensation
Tip: The Trochoidal/HSM Calculator works out the chip thinning compensation automatically.
As soon as the radial depth of cut ae is smaller than 50% of the cutter diameter, an effect that many overlook comes into play: chip thinning compensation. With a small radial depth of cut, the cutting edge touches the material only over a short arc. As a result, the chip actually removed is thinner than the set feed per tooth (fz), so the cutting edge shaves instead of cutting.
The consequence is treacherous: if you do not raise the feed rate at a small ae, you run with a chip that is too thin. The cutting edge then rubs more than it cuts, generates heat and wears faster, which is the same effect as with a feed rate that is generally too low. To keep the cutting edge at the desired effective chip thickness, fz is corrected according to the following relationship:
fz corrected = fz × d / (2 × √( ae × (d − ae) ))
In practice, this means:
- ae = 50% of d (rule-of-thumb maximum from the depth-of-cut rule above): no correction needed, factor ≈ 1.0.
- ae = 25% of d: factor ≈ 1.15, so the feed rate may be about 15% higher.
- ae = 10% of d: factor ≈ 1.67, so the feed rate may be around 67% higher.
Trochoidal milling (HSM) is based on exactly this principle: with a very small ae, but a large cutting depth ap and a correspondingly raised feed rate, the thermal load stays low and tool life stays high. It is important that your machine and spindle can also deliver the higher feed rate cleanly; otherwise, stick to conservative values from the cutting data calculator. Here too, increase gradually and check the chip formation.
Frequently Asked Questions
How do I calculate the optimum spindle speed for my CNC milling cutter?
You calculate the spindle speed with the formula: n = (Vc × 1000) / (π × d). Here, Vc is the material-dependent cutting speed and d is the cutter diameter. For a 6 mm cutter in aluminium (Vc=200), this gives about 10,600 rpm.
What happens with an incorrect feed rate?
A feed rate that is too low creates friction instead of cutting: the cutter gets hot and wears quickly. A feed rate that is too high overloads the tool and the machine and can cause cutter breakage. The optimum feed rate depends on the material, tool and machine.
Do the cutting data apply to all CNC milling machines?
The table values are guideline values for typical CNC gantry mills with solid carbide cutters. Depending on machine rigidity, spindle power and tool quality, the optimum values may differ. Start conservatively and optimise gradually.
0 comments