Cutting data calculator
Spindle speed, feed rate and metal removal rate for turning and milling. With guide values for eight material groups, theoretical roughness and the complete working.
Guide value vc 180 to 350 m/min · f 0.1 to 0.4 mm/rev · coated carbide
Formulas at a glance
The formulas the calculator uses, each with a worked example.
How to calculate spindle speed
n in 1/min, vc in m/min, D in mm. Example: vc 200 m/min on a Ø40 gives 200 · 1000 / (π · 40) = 1,592 1/min. The factor 1000 converts metres to millimetres.
How to calculate cutting speed
The inverse, for when the spindle speed is fixed. Example: Ø40 at 1,592 1/min gives π · 40 · 1,592 / 1000 = 200 m/min.
Feed rate in turning
f in mm per revolution, vf in mm/min. Example: f 0.2 mm at 1,592 1/min gives 318 mm/min.
How to calculate feed rate in milling
fz is the feed per tooth, z the number of flutes. Example: a four-flute Ø10 end mill at vc 150 m/min runs at 4,775 1/min, and with fz 0.05 mm that gives 0.05 · 4 · 4,775 = 955 mm/min.
How to calculate metal removal rate
Q in cm³/min, left for turning, right for milling. Turning example: vc 200 m/min, ap 2 mm and f 0.2 mm give 80 cm³/min. The removal rate shows whether a roughing strategy makes use of the machine power.
Roughness from feed and corner radius
Theoretical values for standard inserts, f and r in mm, multiply the result by 1000 for µm. Example: f 0.2 mm and r 0.8 mm give Rt 6.25 µm and Ra 1.6 µm. Measured values are usually slightly higher.
Guide values by material group
Ranges for carbide with coolant, cross-checked against the catalogues of Sandvik Coromant, Garant, Kennametal and Gühring. Steel, stainless steel, cast iron and titanium with coated grades, aluminium, brass and plastics with sharp, uncoated carbide. Milling feeds apply to solid carbide end mills Ø8 to Ø16 mm, smaller cutters need smaller values. The tool manufacturer specification always takes precedence. The ISO group is the letter under which the values appear in tool catalogues.
| Material | ISO | Turning vc (m/min) | f (mm/rev) | Milling vc (m/min) | fz (mm) |
|---|---|---|---|---|---|
| Structural steel S235, C45, 11SMnPb30 coated carbide | P | 180 to 350 | 0.1 to 0.4 | 150 to 250 | 0.04 to 0.1 |
| Q&T steel 42CrMo4, 34CrNiMo6 coated carbide | P | 120 to 250 | 0.1 to 0.35 | 120 to 180 | 0.03 to 0.08 |
| Stainless steel 1.4301, 1.4404, 1.4571 coated carbide | M | 120 to 250 | 0.1 to 0.3 | 70 to 120 | 0.03 to 0.07 |
| Cast iron EN-GJL-250, EN-GJS-400 coated carbide | K | 150 to 400 | 0.1 to 0.4 | 140 to 220 | 0.05 to 0.1 |
| Aluminium EN AW-6082, EN AW-7075 uncoated carbide | N | 400 to 1,000 | 0.1 to 0.4 | 300 to 800 | 0.05 to 0.12 |
| Brass CuZn39Pb3, CW614N uncoated carbide | N | 200 to 500 | 0.1 to 0.3 | 120 to 250 | 0.04 to 0.1 |
| Titanium Ti6Al4V (3.7165) coated carbide | S | 45 to 90 | 0.1 to 0.25 | 30 to 60 | 0.03 to 0.06 |
| Plastics POM, PA6, PEEK uncoated carbide | N | 150 to 500 | 0.1 to 0.3 | 130 to 300 | 0.05 to 0.15 |
Why spindle speed depends on diameter
The cutting speed vc is the speed at which the cutting edge moves through the material. It depends on the workpiece material and the cutting material, not on the machine. Spindle speed is only the means of reaching it: a point on the circumference travels π times D per revolution. A Ø10 therefore needs four times the spindle speed of a Ø40 to reach the same cutting speed.
In turning, the diameter that counts is the one being cut right now. When facing towards the centre it drops to zero, and the spindle speed would have to rise without limit. That is why facing uses constant surface speed (G96) with a spindle speed limit, G50 on Fanuc and LIMS on Siemens. The field “Max. spindle speed” in the calculator reproduces exactly that.
In milling, D is the cutter diameter. The feed rate follows from the feed per tooth fz, the number of flutes and the spindle speed. fz is the real control variable. If it is too small, the edge rubs instead of cutting and wears quickly. If it is too large, the edge chips.
From the shop floor: With small cutters the spindle often cannot reach the calculated speed. Keep the feed per tooth and accept the lower cutting speed, rather than raising fz to rescue the feed rate. A cutter forced to take chips that are too thick breaks sooner than one running a little too slowly.
Frequently asked questions
How do you calculate spindle speed?
Spindle speed equals cutting speed times 1000 divided by pi times diameter. For vc 200 m/min and a Ø40 that is 200 times 1000 divided by 125.7, roughly 1,592 revolutions per minute. The factor 1000 converts metres to millimetres.
What cutting speed for stainless steel?
For austenitic stainless steel such as 1.4301 (304) or 1.4404 (316L) with coated carbide, 120 to 250 m/min in turning and 70 to 120 m/min in milling. Stainless steel work-hardens during machining, so run with sufficient feed instead of letting the edge rub.
How do you calculate feed rate in milling?
Feed rate equals feed per tooth times number of flutes times spindle speed. A four-flute cutter with fz 0.05 mm at 4,775 1/min runs at 0.05 times 4 times 4,775, roughly 955 mm/min.
Which diameter counts in turning?
The diameter the cutting edge is working on. In longitudinal turning it stays the same, in facing it changes continuously. Modern controls therefore keep the cutting speed constant (G96) and adjust the spindle speed up to a set maximum.
How are feed and surface finish related?
The theoretical peak-to-valley height is feed squared divided by eight times the corner radius. With f 0.2 mm and r 0.8 mm that is 6.25 µm, and Ra is about 1.6 µm. Double the feed gives four times the roughness, double the corner radius halves it. This applies to standard inserts. Wiper inserts reach roughly half the roughness at the same feed.
Why do manufacturer values differ from the table?
The table combines the data of several manufacturers into ranges, and they vary widely: for aluminium Sandvik quotes up to 2,000 m/min, Garant 400 to 700. Edge geometry, coating, clamping rigidity, overhang and the required tool life all shift the right value. Start in the middle of the range, then let chip form and wear pattern decide.
Request parts
Send a drawing or STEP file. We check manufacturability and reply within 24 hours.
Start request