Cutting data calculator for turning, milling and drilling
The calculator determines spindle speed n, feed rate vf, material removal rate Q and machining time t_h for the three basic operations. Reference values for the cutting speed vc are stored per material group and cutting tool; for turning the cutting force can additionally be estimated after Kienzle. All reference values are starting points for average conditions, and the tool manufacturer's data for the specific tool takes precedence.
Calculate cutting data
Approximation without correction factors. Real forces typically 20…50 % higher due to wear; kc1.1/mc scatter between sources (±20 %).
Composition of the feed path L
Cutting force and power (Kienzle)
Formulas and fundamentals
Kinematics: From the cutting speed vc and the governing diameter the spindle speed follows as n = vc·1000/(π·d). For turning d is the workpiece diameter, for milling and drilling the tool diameter. The factor 1000 converts metres to millimetres. Conversely, a given spindle speed yields vc = π·d·n/1000.
Feed rate: For turning and drilling vf = f·n with the feed per revolution f. For milling the teeth add up: vf = fz·z·n with the feed per tooth fz and the number of teeth z. For z = 1 the milling formula reduces to the turning formula.
Material removal rate: For turning Q = ap·f·vc, for milling Q = ap·ae·vf/1000, for drilling into solid Q = π/4·d²·vf/1000 = d·f·vc/4. Each result is directly given in cm³/min. The drilling formula represents the geometrically removed volume; a simplification common in some reference books yields twice this value.
Machining time: t_h = L·i/vf with the total feed path L per pass and the number of passes i. The path L consists of approach, machining length and overtravel. For drilling the lead-in of the drill point l_s = d/(2·tan(σ/2)) is added, which for the standard point angle of 118° is about 0.3·d. For longitudinal turning with an oblique lead angle κ < 90° the lead-in path l_ak = ap/tan κ is added as well, the distance the edge travels until full depth of cut; at κ = 90° it is zero. For milling the cutter diameter is added or subtracted depending on the path convention.
Cutting force after Kienzle (turning): From the chip thickness h = f·sin κ and the chip width b = ap/sin κ the specific cutting force kc = kc1.1/h^mc follows, and from it the cutting force Fc = A·kc with the chip cross section A = ap·f. The cutting power is Pc = Fc·vc/60000 in kW, the required machine power P_M = Pc/η, and the spindle torque M = Fc·d/2000 in Nm. The values kc1.1 and mc depend on the material and scatter noticeably between sources.
Worked example
Example turning an S235 shaft of Ø 60 mm, coated carbide: With vc = 200 m/min the spindle speed is n = 200·1000/(π·60) = 1061 rpm. With a feed f = 0.3 mm the feed rate is vf = 0.3·1061 = 318 mm/min. With a depth of cut ap = 2.5 mm the material removal rate is Q = 2.5·0.3·200 = 150 cm³/min.
For a turning length of 120 mm with 2 mm approach and overtravel each, L = 124 mm and the machining time t_h = 124/318 = 0.39 min, about 23 seconds per pass. Adding the cutting force for 42CrMo4 (kc1.1 = 2500 N/mm², mc = 0.26) at ap = 3 mm, f = 0.3 mm and κ = 90° gives kc = 3419 N/mm², Fc = 3077 N and a cutting power Pc = 7.7 kW.
Frequently asked questions
Where do the cutting speed reference values come from?
The vc ranges are consolidated from several public sources (reference books, manufacturer catalogues, independent calculators) per material group and cutting tool and apply to average conditions. They are deliberately given as ranges because grade, coating, geometry, cooling and machine stability shift the value considerably. The manufacturer's data for the specific tool always takes precedence.
Which diameter should I enter?
For turning it is the workpiece diameter where the cut takes place (for shoulders the current one). For milling and drilling it is the tool diameter. This distinction determines the correct spindle speed, because the cutting speed always applies at the outer cutting diameter.
How accurate is the cutting force after Kienzle?
The Kienzle approach is a proven approximation for the straight main cutting edge. The correction factors for rake angle, cutting speed, wear and chip compression are not active in this calculator. Real forces are typically 20 to 50 percent higher due to tool wear, and the values kc1.1 and mc scatter by about ±20 percent between sources and batches. The values are suitable for design and machine checks, not as measured data.
Why does my calculated spindle speed differ from the machine step?
The calculator outputs the exact target speed from the cutting speed. Older machines only have fixed speed steps. Therefore the nearest step of a preferred-number series is additionally shown as a hint. On the chosen step a slightly different actual cutting speed results.
What does the lead-in path when drilling mean?
The drill point must first fully engage before the full diameter cuts. This lead-in path is l_s = d/(2·tan(σ/2)) and gives about 0.3·d for the standard point angle of 118°. For short holes this accounts for a considerable part of the time; the calculator includes it automatically.
What is the difference between the milling path conventions?
When passing over a surface the cutter must stand clear in front of and behind the workpiece, so the cutter diameter is added to the path. For a closed slot the cutter centre travels one diameter less, so it is subtracted. In direct mode the entered path is taken unchanged as the path of the cutter centre.