Sheet Metal Guides

Bend Deduction vs Bend Allowance: Diagram & Examples

Distinguish tangent lengths, outside mold-line legs, bend allowance and deduction. Compare equivalent flat-length methods with a non-90° worked example.

Published September 16, 2026Updated October 8, 2026Editorial method

Bend allowance and bend deduction are two ways to account for the same formed bend. Bend allowance describes neutral-axis arc length; bend deduction is the amount subtracted from the sum of outside flange dimensions to obtain the flat length.

Quick answer

Outside setback = tan(A ÷ 2) × (R + T)

Bend deduction = 2 × outside setback − bend allowance

In this guideThree terms Worked example Which workflow Common errors

Bend allowance, setback, and deduction

Bend allowance (BA) is the neutral-axis length through the bend. Outside setback (OSSB) is the distance from the mold-line intersection to the bend tangent along an outside leg. For a bend angle A, inside radius R, and thickness T:

Outside setbackOSSB = tan(A / 2) × (R + T)A is the bend angle; use a consistent angle convention

Bend deductionBD = 2 × OSSB − BABA = A_rad × (R + K × T)

Worked 90-degree example

Use thickness 2.0 mm, inside radius 2.0 mm, K-factor 0.40, and a 90° bend.

BA = 1.5708 × (2 + 0.40 × 2) = 4.398 mm.
OSSB = tan(45°) × (2 + 2) = 4.000 mm.
BD = 2 × 4.000 − 4.398 = 3.602 mm.

If the two outside flange dimensions are 50 mm and 40 mm, the flat length is 50 + 40 − 3.602 = 86.398 mm. If the drawing instead provides tangent lengths, add bend allowance to those straight lengths rather than subtracting bend deduction from outside dimensions.

Choose the formula that matches the drawing

Dimension basis	Flat-length workflow
Tangent-to-tangent straight lengths	Add bend allowance
Outside mold-line flange dimensions	Subtract bend deduction
Validated shop bend table	Use the table’s stated convention

For multiple bends, work through each bend using the same drawing convention and validated process data. CAD systems may expose K-factor, bend allowance, bend deduction, or a bend table; verify which field the software expects.

Common sources of flat-pattern error

Using the included angle where the formula expects bend angle, or vice versa.
Combining outside dimensions with a tangent-length formula.
Using punch-tip radius instead of achieved inside radius.
Reusing a K-factor after changing material, grain direction, V-opening, or bend method.
Rounding each intermediate value too early.
Treating a theoretical result as final without a test bend and measurement plan.

Technical references

WILA — V-opening effects on product radius and flat pattern

Published and formula-checked by MfgWorkbench. Last reviewed September 15, 2026. See our editorial method.

Keep the dimension basis visible

Original bookkeeping diagram. Outside-leg dimensions are measured to the virtual sharp; tangent lengths stop at the bend.

SOLIDWORKS documents the two flat-length methods and the virtual-sharp basis for deduction. The diagram shows why adding BA to outside legs counts the setback portions incorrectly.

For a non-right-angle comparison, take T = 1.5 mm, R = 3 mm, K = 0.40 and bend angle A = 60° (included angle 120°). BA = 3.7699 mm; each OSSB = tan(30°) × 4.5 = 2.5981 mm; therefore BD = 2 × 2.5981 − 3.7699 = 1.4262 mm.

If outside legs are 30 mm and 45 mm, flat length is 30 + 45 − 1.4262 = 73.5738 mm. The equivalent tangent calculation is (30 − 2.5981) + (45 − 2.5981) + 3.7699 = the same 73.5738 mm. Equality is a useful check that the two methods used the same geometry.

For several bends, establish a consistent dimension chain and apply each bend’s own radius, angle and validated correction. Do not subtract every visible bend deduction from an arbitrary overall dimension. The numbers here are analytical examples, not measured shop capability.

Content updated October 8, 2026. Sources and numerical examples are explained above; examples are not production test results. Editorial method · Report a correction.