Machining formula reference
Calculate spindle speed and feed rate from cutting speed, tool diameter and tooth count, with typical starting ranges per material.
Manufacturer data · Record tool and material scope · unit: m/min
Starting ranges for a general setup. The tooling supplier data for the exact insert always governs the released values.
| Material | Carbide Vc (m/min) | HSS Vc (m/min) | fz Ø≤6 (mm/tooth) | fz Ø6–12 (mm/tooth) | fz Ø12–25 (mm/tooth) | Note |
|---|---|---|---|---|---|---|
| Aluminium 6061-T6 | 300 – 600 | 60 – 120 | 0.02 | 0.05 | 0.1 | Excellent chip formation; watch for built-up edge on small depths |
| Aluminium 7075-T6 | 250 – 500 | 50 – 100 | 0.02 | 0.05 | 0.1 | Higher strength than 6061 – reduce the upper end |
| Mild steel S355 / AISI 1045 | 120 – 220 | 20 – 40 | 0.02 | 0.04 | 0.08 | General purpose machining steel |
| Alloy steel AISI 4140 / 42CrMo4 | 100 – 180 | 15 – 35 | 0.02 | 0.04 | 0.08 | Prefer a positive feed to avoid rubbing |
| Stainless steel 304 / 316L | 80 – 150 | 10 – 25 | 0.02 | 0.04 | 0.08 | Work hardening – keep the feed above the minimum |
| Tool steel D2 (hardened) | 40 – 90 | 8 – 20 | 0.01 | 0.03 | 0.06 | Use a coated carbide or CBN when hardened |
| Tool steel H13 (mould steel) | 60 – 120 | 8 – 20 | 0.02 | 0.04 | 0.07 | Common for injection-mould tooling |
| Titanium Ti-6Al-4V | 40 – 90 | 5 – 12 | 0.02 | 0.04 | 0.07 | Low thermal conductivity – high coolant flow needed |
| Brass C360 / free-machining | 200 – 400 | 40 – 80 | 0.02 | 0.05 | 0.1 | Very machinable – can run high speeds |
| Copper C110 | 100 – 250 | 15 – 30 | 0.02 | 0.05 | 0.1 | Sticky build-up – use a sharp edge |
| Nickel Inconel 718 | 20 – 50 | 3 – 8 | 0.02 | 0.04 | 0.07 | Severe work hardening – keep the load stable |
| Cast iron GG25 / EN-GJL-250 | 80 – 150 | 10 – 25 | 0.03 | 0.06 | 0.12 | Dry cutting is possible with coated carbide |
| Acetal / POM | 150 – 400 | 30 – 80 | 0.05 | 0.1 | 0.15 | Low friction and a very good surface finish |
| PEEK / PPS (engineering plastics) | 100 – 250 | 15 – 30 | 0.05 | 0.08 | 0.12 | Avoid dwell time – the material rubs and melts |
Machining handbook · Current edition · unit: Mixed units
The formulae behind the calculator. Keep the unit of every term visible when you copy them into a machining sheet.
| Quantity | Symbol | Formula | Unit | Typical range | Note | Source |
|---|---|---|---|---|---|---|
| Cutting speed | Vc | Vc = π × D × n / 1000 | m/min | 20 – 400 | The surface speed at the cutting edge | Machining handbook |
| Spindle speed | n | n = 1000 × Vc / (π × D) | rev/min | 100 – 20 000 | Revolutions per minute at the spindle | Machining handbook |
| Feed per tooth | fz | fz = Vf / (n × z) | mm/tooth | 0.01 – 0.30 | The advance of one tooth per revolution | Machining handbook |
| Feed rate | Vf | Vf = fz × z × n | mm/min | 10 – 5 000 | The advance of the tool per minute | Machining handbook |
| Material removal rate | MRR | MRR = Vc × fz × z / 1000 | cm³/min | 5 – 2 000 | Volume of material removed per minute | Machining handbook |
| Depth of cut | ap | ap = (height of the cut) | mm | 0.1 – 10 | Axial depth removed in one pass | Machining handbook |
| Engagement width | ae | ae = width of the cut | mm | 0.1 – 50 | Radial or axial width of the cut | Machining handbook |
| Tool life (Taylor) | T | T = C × Vc^m × fz^n | min | 10 – 240 | Empirical relationship – the constants are tool specific | Machining handbook |
| Steady-state chip load | h | h = fz × cos(kr) × √(ae / ap) | mm | 0.005 – 0.5 | Average chip thickness for a round insert | Machining handbook |
The calculator uses only the values you enter, so it cannot tell you whether the cutting speed is safe for your machine, the tool and the setup. The reference table gives the typical starting ranges for common work materials and the formulae behind the calculator. Start at the lower end of the range and raise it step by step.
Reference source
Machining formula reference
Vc is the cutting speed at the cutting edge, measured in m/min. fz is the chip load, the advance per tooth per revolution in mm. Vf is the feed rate in mm/min. Vf is the one that ends up on the machine, and it follows from Vf equals fz multiplied by the number of teeth multiplied by the spindle speed.
n equals 1000 multiplied by Vc divided by pi multiplied by the tool diameter. For a 10 mm carbide end mill at Vc 200 m/min that gives about 6360 rev/min. Always enter the actual tool diameter, and remember that the machine has a maximum speed that can force you to reduce Vc.
Start near the middle of the range for the material and the tool diameter, then adjust. Roughing can run at the upper end, finishing at the lower end, and a stable machine with a rigid setup can take more. Change one variable at a time so you know what fixed the problem.
Because the ranges are typical averages for a general setup. A long tool overhang, a thin wall, an older machine or an unfamiliar material all push the real cutting point down. Starting low keeps the tool alive and gives you a stable baseline to raise from.
A bigger tool can usually take a higher chip load per tooth, because the force is spread over more teeth and a bigger contact area. But the available spindle power also grows with diameter, so the useful reference is the fz columns per diameter band rather than a single number.
When the machine starts to lose finish, when the tool load grows on the upswing, or when the chip gets too thick to evacuate. A very rough first cut is fine, but a thick chip over a long pass ties up the machine and destroys the tool. Reduce the depth of cut and keep the feed steady.
No. They are general starting ranges for a common geometry. Your tooling supplier publishes the data for the exact insert, and for coated grades on hardened steel or titanium the difference can be large. Use the table to plan the job, then use the supplier data to release it.
Send the drawing and the requirements to Evefab’s engineering team. We reply with manufacturability feedback, not just a price.
