Turning Depth of Cut: Radial vs Diameter Examples

For straight external turning, radial depth of cut is half the reduction in diameter: depth of cut = (starting OD − finished OD) ÷ 2. Removing 0.100 inch from a diameter means a 0.050-inch radial cut. Confusing those quantities can double the intended cut.

Why turning depth of cut uses radius

A diameter spans both sides of the centreline. When a cylindrical surface moves inward by one unit of radius, its diameter decreases by two units. ISCAR’s cutting-data guide gives the external longitudinal turning equation as half the difference between unmachined and machined diameters. This guide applies that geometry to pass planning; it does not choose a suitable cut for your insert or machine.

Inch example: from 2.000 to 1.800 OD

The diameter reduction is 2.000 − 1.800 = 0.200 inch. Total radial stock is therefore 0.200 ÷ 2 = 0.100 inch. Two equal radial cuts of 0.050 inch would geometrically reach 1.800 OD: the first changes the diameter to 1.900, and the second to 1.800. This is an arithmetic example, not a recommended pass schedule.

Metric example: reserve a finishing allowance

Start with 60 mm OD and finish at 50 mm. Total radial stock is (60 − 50) ÷ 2 = 5 mm. Suppose the process plan reserves 0.5 mm radially for finishing. That leaves 4.5 mm radial stock for roughing. If the chosen roughing depth is at most 2 mm radially, the geometric minimum is ceil(4.5 ÷ 2) = three roughing passes.

One possible diameter sequence is 60 → 56 → 52 → 51 mm, followed by the finishing pass to 50 mm. The third roughing pass removes only 0.5 mm radially. Equalising roughing passes is another possible planning choice; the appropriate strategy depends on the tooling and process. Always check whether an allowance field means radial stock or diameter stock.

For boring, reverse the diameter subtraction

When enlarging an existing cylindrical hole, the final ID is larger. Radial stock removed is (finished ID − starting ID) ÷ 2. Enlarging a 20 mm bore to 24 mm removes 2 mm radially. ISCAR lists this internal-turning form separately. These equations describe stock between coaxial cylindrical surfaces; they do not describe the axial depth of a drilled hole.

Use pass count in a runtime estimate

More passes usually add more feed travel and repositioning moves. For a rough estimate, enter radial depth and finish allowance in the lathe cycle-time estimator. Use the turning RPM and feed calculator for a chosen diameter, and read the cutting-time and batch-time examples for the distinction between cutting and non-cutting time.

A pass count alone does not establish a safe process or exact runtime. Actual stock variation, stepped lengths, tool access, chip control, rigidity and machine motion also matter. Select cutting data from the exact insert and holder manufacturer’s guidance for the material and setup.

Common questions

Is a 0.050-inch turning cut radial or on diameter?

The phrase alone is ambiguous. A radial depth of 0.050 inch reduces OD by 0.100 inch. A diameter reduction of 0.050 inch corresponds to 0.025 inch radial depth. State the convention explicitly.

Does diameter-mode X programming change the geometry?

No. Diameter mode changes how coordinates are expressed. The radial material removed is still half the change in diameter. Check how your control defines each cycle’s depth and allowance fields separately.

Manufacturer reference

ISCAR cutting-data guide: external turning and boring depth-of-cut equations. Worked dimensions and pass sequences above are original illustrative calculations.