Machining Speed, Feed and Cycle Time Formulas

Start with consistent units

The formula sheet uses cutting speed vc in metres per minute, machined diameter Dm in millimetres, spindle speed n in revolutions per minute, feed fn in millimetres per revolution and machined length lm in millimetres. Keeping that unit set together is essential. The factor 1000 in the speed equation converts millimetres to metres. If a drawing or machine control uses inches, convert the inputs first or use a matching imperial formula sheet; mixing inch diameter with the metric equation creates a result that is wrong by a factor of 25.4.

For a 50 mm workpiece at 2000 rev/min, vc = π × 50 × 2000 / 1000 = about 314 m/min. Reversing the equation, a 50 mm diameter at 200 m/min requires about 1273 rev/min. These examples are kinematic conversions. They do not indicate whether a tool, material or machine should run at that speed.

Machined diameter is the diameter at the cutting edge for the operation being calculated. On a turning pass, that may change as the workpiece diameter changes. A constant surface-speed control varies spindle rpm to maintain vc, subject to a programmed maximum speed. A fixed-rpm operation does not preserve cutting speed across changing diameters, so understand the control mode before interpreting a single rpm value.

Estimate engagement time

The turning engagement equation is Tc = lm/(fn × n). Feed per revolution multiplied by spindle speed gives axial feed per minute in mm/min. Dividing the engaged length by that feed gives minutes. For a 120 mm cut at 0.20 mm/rev and 1000 rev/min, the feed is 200 mm/min and ideal cutting time is 0.60 min, or 36 seconds. Use the engaged travel, including any allowance that the machining plan counts as cutting travel.

This equation estimates time while the tool is engaged at steady feed. It excludes approach, retract, acceleration, tool changes, indexing, inspection, loading and other machine delays. A complete cycle-time estimate must account for those operations separately. Interrupted cuts, changing feed, multiple passes and variable spindle speed also need segmented calculations instead of one average feed and rpm.

Estimate material removal and power

For the turning geometry shown by Sandvik, Q = vc × ap × fn gives metal removal rate in cubic centimetres per minute when vc is in m/min and ap and fn are in millimetres. A 200 m/min cut with 2 mm depth and 0.20 mm/rev feed yields 80 cm³/min. Treat this as a geometry-based rate under the equation’s turning assumptions; it does not account for entry effects or a changing cut.

The net-power equation adds specific cutting force kc: Pc = vc × ap × fn × kc / (60 × 10³). Sandvik lists kc in N/mm² and output power in kW. The conversion constant carries the unit conversions from the selected inputs. Specific cutting force varies with material and chip conditions, so an appropriate toolmaker value is required. A result is an estimate of cutting power, not a motor sizing approval or a guarantee that the machine can sustain that load.

Keep chip geometry definitions clear

Average chip thickness is related to feed and entering angle by hm = fn × sin(KAPR). The entering angle changes how a given feed becomes chip thickness and affects the load presented to an insert. Sandvik’s sheet defines KAPR in degrees. Use a calculator configured for degrees when evaluating the sine, and do not substitute an insert’s nose radius or a different angle definition without checking the tool geometry.

Feed per revolution, feed per tooth, table feed and chip thickness describe different quantities. They have different units and belong to different operation formulas. The table identifies fn as mm/rev. A milling feed per tooth cannot be inserted directly into this turning expression, and spindle rpm should not be confused with surface speed. Always read the variable definition alongside the equation.

Apply the results to the actual setup

Use these equations to translate known cutting conditions into a speed, time, rate or power estimate. Select recommended cutting data from the material and cutting-tool supplier for the exact alloy, tool grade, geometry, coating, coolant, depth and machine. Check spindle-speed limits, workholding, rigidity and tool overhang before applying the result. Tool life, surface finish, chip control and safety depend on conditions that these relationships do not capture.

A useful calculation record names the operation, material, tool, diameter, cutting speed, feed per revolution, depth and unit system. Keep full precision during intermediate steps and round only the displayed result to a practical setting. Compare a calculated value with machine and tooling limits, and verify the first part through inspection. If the geometry or cutting mode changes during a cycle, calculate each segment separately and sum the engagement times.

Source and scope

Formula source: Sandvik Coromant, formulas and definitions for turning (metric).