車削加工計算公式大全：切削速度、進給量與表面粗糙度解析｜車削技術資訊

Core turning calculations cover cutting power (Pc), cutting speed (Vc), feed (f), machining time (Tc) and surface roughness (h). These formulas quickly assess machine load, efficiency and surface quality. This guide organises the general formulas and their factors to help optimise cutting conditions and reduce tool wear.

Required power Pc formula and worked example: Pc = ap x f x vc x Kc / (60 x 10^3 x eta) kW. The example uses 3 mm depth of cut, 120 m/min cutting speed and 0.2 mm/rev feed on mild steel (Kc = 3100 MPa, 80% machine efficiency), giving 4.65 kW

1. Why These Calculations Matter

They assess machining load, predict efficiency and control surface quality, and are used for tool selection, cutting-parameter setting and cost control. Mastering them balances efficiency against tool life.

Tool-maker specific cutting force Kc reference tables (two stacked tables). Rows list mild steel, medium-hard steel, hard steel, tool steel, chrome-manganese, chrome-molybdenum, chrome-nickel-molybdenum steels, chilled iron, inoculated iron and grey iron with their hardness; the three right-hand columns give Kc under different conditions, roughly 1330 to 4510 MPa across the tables

2. General Formulas

Item	General formula	Symbols
Cutting speed Vc	Vc = π·Dm·n / 1000 (m/min)	Dm dia mm, n rpm
Spindle speed n	n = 1000·Vc / (π·Dm) (rpm)	from target Vc
Cutting power Pc	Pc = ap·f·vc·Kc / (60×10⁶) (kW)	ap mm, f mm/rev, Kc N/mm²
Machining time Tc	Tc = lm / (f·n) (min)	lm length mm
Theoretical roughness h	h ≈ f² / (8·R) (mm)	R nose radius mm

These are general reference formulas; actual speeds/feeds should follow the tool catalogue and the Turning Cutting Conditions Guide, not applied blindly.

Cutting speed vc formula and worked example: vc = pi x Dm x n / 1000 (m/min). The example uses 700 rpm spindle speed and 50 mm workpiece diameter, giving 110 m/min, with a diagram of the tool cutting the rotating bar

3. Specific Cutting Force (Kc)

Different materials have different cutting resistance; harder material means higher Kc and greater power demand. Typical reference ranges (vary with grade and chip thickness):

Material	Kc typical ref (N/mm²)
Mild steel	~2500–2900
Medium-carbon steel	~2900–3300
Alloy steel	~3000–4500
Cast iron	~1300–2100

The table gives practical Kc values from tool-maker cutting data (matching the maker chart in this section and the power example that uses Kc = 3100 MPa for mild steel); they already include real chip thickness effects. Typical ranges — follow the catalogue or standard. Note this is not the same figure as kc_1.1: kc_1.1 is the reference value at 1 mm chip thickness and 0° rake (steel about 1350–1900, grey cast iron about 1150–1350). Actual kc rises as chip thickness falls (kc = kc_1.1 / h^mc, mc about 0.2–0.28; roughly 1.7–1.8x at h = 0.1 mm). Much smaller figures seen elsewhere are usually kc_1.1, not errors.

Feed per revolution f formula and worked example: f = l / n (mm/rev). The example uses 500 rpm spindle speed and 120 mm/min cutting length per minute, giving 0.24 mm/rev

4. Cutting Speed (Vc) and Feed (f)

Cutting speed is the relative speed of tool and workpiece, set by diameter (Dm) and speed (n), used to set a sensible rpm and control tool life. Feed is the advance per revolution, affecting roughness and load: more feed raises efficiency but lowers surface quality.

Diagram of feed per revolution: shows workpiece rotation n, cutting length per minute l and feed per revolution f, with the turning tool leaving a helical tool mark on the surface; annotated feed per revolution 0.24 mm/rev

5. Machining Time (Tc) and Roughness (h)

Machining time is the time to finish a cut, set by length and feed rate, used for time estimation and scheduling. Theoretical roughness depends on feed (f) and nose radius (R): more feed → worse roughness, larger radius → better roughness.

Machining time Tc formula and worked example: Tc = lm / l (min). The example uses a 100 mm long workpiece at 1000 rpm and 0.2 mm/rev feed; cutting length per minute is first found as 200 mm/min, giving 0.5 minutes (30 seconds)

6. Example and Parameter Adjustment

If machining time is too long, parameters are often too conservative — raise feed or depth moderately, while checking that power stays within the machine's capacity and roughness still meets the requirement. Power calculation shows whether the machine is overloaded.

Theoretical surface roughness h formula and worked example: h = f^2 / (8 x RE) x 1000 (micrometre). The example uses 0.8 mm nose radius and 0.2 mm/rev feed, giving 6.25 micrometre, with two diagrams comparing how a larger feed leaves a taller residual tool mark

7. Engineering Key Points

The key control parameters are cutting speed vc, feed f and depth ap; the optimisation goals are stable machining, longer tool life and higher productivity. For nose radius and angle effects see the Turning Tool Nose Radius Guide and Turning Tool Rake & Clearance Guide.

For the full reading guide on this topic, see Turning Toolpaths: The Complete Guide.

FAQ

Q: How to convert speed and rpm?

Use Vc = π·Dm·n/1000, or invert n = 1000·Vc/(π·Dm). Since turning diameter changes, a larger diameter has higher surface speed at the same rpm, so finishing small diameters often needs higher rpm to hold Vc.

Q: How to reduce surface roughness?

Theoretical roughness h≈f²/(8R), so smaller feed f or larger nose radius R improves it. Finishing uses small feed and larger R, but too large an R raises radial force and can cause chatter, so balance with rigidity.

Q: How to pick Kc?

Kc varies with material and chip thickness; the values here are typical references. For accurate power, use the tool maker's Kc data for that material and feed rather than a single value.

Q: Power exceeds the machine — now what?

Pc is proportional to ap, f and vc, so reduce depth or feed, or cut in passes. A sharper (positive-rake) insert also lowers cutting force, but keep edge strength and stability in mind.

For the full reading guides on this topic, see Surface Finish: A Complete Reading Guide and Machining Calculation Reading Guide.

Home ＞ Technical Information ＞ Turning Technical Guide ＞ Turning Machining Formulas: Speed, Feed & Surface Roughness