CNC Lathe Feed Rate Calculator

CNC Lathe Feed Rate Calculator

Popular AI Skill PRO

Enter Calculation

Formula

F=Spindle Speed (RPM)×Feed per Rev (mm/rev)Fin/min=F25.4\begin{gathered} F = \text{Spindle Speed (RPM)} \times \text{Feed per Rev (mm/rev)} \\[1.5em] F_{\text{in/min}} = \frac{F}{25.4} \end{gathered}
Show calculation steps (2)
  1. Cutting Speed (m/min and SFM)

    Vc=π×Diameter (mm)×Spindle Speed (RPM)1000SFM=3.28084×Vc\begin{gathered} V_c = \frac{\pi \times \text{Diameter (mm)} \times \text{Spindle Speed (RPM)}}{1000} \\[1.5em] \text{SFM} = 3.28084 \times V_c \end{gathered}

    Vc = pi x D x RPM / 1000; SFM = Vc x 3.28084

  2. Machining Time (min)

    T=Cut Length (mm)Spindle Speed (RPM)×Feed per Rev (mm/rev)T = \frac{\text{Cut Length (mm)}}{\text{Spindle Speed (RPM)} \times \text{Feed per Rev (mm/rev)}}

    Cut length divided by feed rate F = RPM x feed; zero if feed rate or length is not positive

Usage stats

Advertisement

Results

Feed Rate
240
mm/min
Cutting Speed (m/min) 188.5
Feed Rate (in/min) 9.45
Cutting Speed (SFM) 618.42
Machining Time for Cut Length (min) 0.42

Report an error on this page

What is the CNC lathe feed rate calculator?

This calculator converts the basic turning parameters of a CNC lathe into the numbers a machinist actually programs: the linear feed rate in mm/min and the surface cutting speed in m/min. It also gives imperial equivalents (in/min and SFM) and an estimated cutting time for a pass of a given length. The formulas are universal geometry and kinematics, so they apply to any lathe.

Lathe workpiece with rotation N, tool feed F and diameter D marked
Spindle speed N, workpiece diameter D and the tool's feed motion F on a turning operation.

How to use it

Enter the workpiece diameter in millimetres, the spindle speed in RPM and the feed per revolution in mm/rev. Optionally enter the length of the cut to estimate machining time. The calculator returns the feed rate, cutting speed and time instantly. If your control runs in G99 (feed per revolution) you program f directly; in G98 (feed per minute) you program the calculated feed rate.

The formulas explained

Feed rate is the distance the tool travels per minute:

$$F = N \times f$$

where \(N\) = spindle speed in RPM and \(f\) = feed per revolution in mm/rev. Cutting speed is the speed of the surface passing the tool edge:

$$V_c = \frac{\pi \times D \times N}{1000}$$

where \(D\) = diameter in mm, giving \(V_c\) in m/min. Cutting time for a pass is \(t = L / F\), with \(L\) the cut length in mm.

Advertisement
Feed per revolution shown as tool advance during one spindle turn
Feed per revolution (f) is the distance the tool advances along the part during one spindle turn.

Worked example

Turning a 50 mm bar at 1200 RPM with a feed of 0.2 mm/rev over a 100 mm length:

$$F = 1200 \times 0.2 = 240\,\text{mm/min}$$$$V_c = \frac{\pi \times 50 \times 1200}{1000} \approx 188.5\,\text{m/min}$$$$t = \frac{100}{240} \approx 0.417\,\text{min}$$

In imperial units that is about 9.45 in/min and 618 SFM.

End view of workpiece showing diameter, rotation and surface cutting speed
Cutting speed V is the surface speed at the tool contact point and depends on diameter and RPM.

Typical Cutting Speeds by Workpiece Material

Cutting speed \(V_c\) is the surface speed at the tool tip. It links diameter and spindle speed: $$V_c = \frac{\pi \cdot D \cdot N}{1000}$$ with \(D\) in mm, \(N\) in RPM and \(V_c\) in m/min. To convert to surface feet per minute, use SFM ≈ m/min × 3.281. The table gives approximate starting ranges for coated carbide inserts in general-purpose turning.

Material Vc, carbide (m/min) Vc, carbide (SFM)
Free-cutting steel (e.g. 11SMn30, 12L14) 200–350 650–1150
Mild / medium carbon steel (approx. C15–C45) 150–250 490–820
Stainless steel 304 (austenitic) 100–180 330–590
Grey cast iron 120–250 390–820
Aluminium alloys 300–800 980–2620
Brass (free-cutting) 200–400 660–1310
Titanium (e.g. Ti-6Al-4V) 40–80 130–260

Note: these are approximate, general starting values. Always follow the insert or tool manufacturer's catalogue data for the specific grade, geometry, coolant and material condition, because that data takes priority over any generic table. Use lower speeds for interrupted cuts, long overhangs or hard material conditions.

Advertisement

Typical Feed per Revolution Ranges

Feed per revolution \(f_r\) (mm/rev) is the distance the tool advances for each spindle turn. The table gives typical ranges for carbide tooling in general turning.

Operation Feed per revolution (mm/rev)
Roughing 0.25–0.50
Semi-finishing 0.15–0.25
Finishing 0.05–0.15
Grooving 0.03–0.15 (smaller for narrow grooves)
Parting off 0.05–0.15 (reduce near the centre)
  • For finishing, keep the feed at or below roughly 50–70% of the insert nose radius. A larger feed leaves visible feed marks and worsens surface finish.
  • The usable feed depends on the insert geometry and grade, the workpiece material, depth of cut, coolant and machine rigidity. Slender or long-overhang workpieces need lower feeds.
  • Check the tool maker's recommended range for the insert you are using.

Comparing Feed and Speed Scenarios

All scenarios use a feed of 0.2 mm/rev and a 100 mm cut length. The formulas are \(F = N \cdot f_r\), \(V_c = \pi D N / 1000\), \(N = 1000\,V_c/(\pi D)\) and cutting time \(t = L / F\).

Scenario Diameter (mm) RPM Feed rate F (mm/min) Vc (m/min) Time for 100 mm
Fixed RPM 20 2000 400 125.7 0.25 min (15 s)
Fixed RPM 50 2000 400 314.2 0.25 min (15 s)
Fixed RPM 100 2000 400 628.3 0.25 min (15 s)
Constant Vc = 200 m/min 20 3183 636.6 200 0.157 min (9.4 s)
Constant Vc = 200 m/min 50 1273 254.6 200 0.393 min (23.6 s)
Constant Vc = 200 m/min 100 637 127.3 200 0.785 min (47.1 s)

Worked check for the 50 mm, constant-Vc row: $$N = \frac{1000 \times 200}{\pi \times 50} = 1273.2\ \text{RPM}, \quad F = 1273.2 \times 0.2 = 254.6\ \text{mm/min}, \quad t = \frac{100}{254.6} = 0.393\ \text{min}$$

Key takeaways: at fixed RPM the feed rate and cutting time do not change with diameter, but the surface speed rises in proportion to diameter. Speeds of 300–600 m/min are only realistic for materials such as aluminium. At constant surface speed, larger diameters need a lower RPM, so the feed rate falls and cutting time grows. This is why CNC lathes offer constant surface speed (CSS) mode, usually with a maximum RPM limit.

FAQ

Why does cutting speed change with diameter?

At constant RPM, a larger diameter moves faster at the surface. With constant surface speed (G96) the control raises RPM as the diameter decreases.

What feed per revolution should I use?

Roughing typically uses 0.2 to 0.4 mm/rev and finishing 0.05 to 0.15 mm/rev, depending on insert nose radius, material and tool maker recommendations.

Does this include acceleration or rapid moves?

No. The time is the pure cutting time at constant feed and ignores tool approach, retracts and tool changes.

Last updated:

Most popular in Industry-Specific

View all Industry-Specific calculators