Sheet-Metal Bend Allowance Calculator

Bend allowance, bend deduction, setback, flat blank length and press-brake force for a sheet-metal bend from the thickness, radius, angle and K-factor.

How it works

When sheet is bent, the outside stretches and the inside is compressed. A line between them, the neutral axis, keeps its length. It lies a fraction K of the thickness in from the inside surface (the K-factor), so the bend takes up a length called the bend allowance.

BA = θ × (r + K T), OSSB = tan(θ ÷ 2) × (r + T), BD = 2 × OSSB − BA, flat = A + B − BD

The force for air bending in a V-die is F = 1.33 × UTS × L × T² ÷ V (a common press-brake chart formula). Check the press rating and the die load rating. The ideas of materials and joining are in Prototyping Techniques and Structures and Strength of Materials.

Worked example

A 2 mm mild-steel sheet is bent through 90° with an inside radius of 2 mm and K = 0.33, with two flanges of 50 mm measured to the outside, 1 000 mm long, in a 16 mm V-die; the tensile strength is 400 MPa.

  • BA = (π ÷ 2) × (2 + 0.33 × 2) = 4.178 mm.
  • OSSB = tan 45° × (2 + 2) = 4.000 mm; BD = 2 × 4 − 4.178 = 3.822 mm.
  • Flat length = 50 + 50 − 3.822 = 96.178 mm.
  • Force = 1.33 × 400 × 1 000 × 2² ÷ 16 = 133 000 N = 133 kN (13.6 tonnes-force). The smallest flange is about 0.7 × 16 = 11.2 mm.

Things to know

The K-factor is empirical: it depends on the material, the thickness, the radius, the die and the bending method (air, bottoming, coining). Bend a test piece and measure to find the value for your tooling.

Measure the flange dimensions to the same reference as the drawing. If the drawing gives inside dimensions, convert them to the outside by adding the thickness.

With a tight inside radius (under one thickness) the metal may crack on the outside of the bend, and the bend line should run across the grain, not along it. Check the minimum bend radius of your material and temper.

The springback of the metal opens the bend slightly after release: press brakes overbend by 1 to 3 degrees for steel, more for stainless and spring-tempered alloys.

Holes and slots need to be at least 2.5 thicknesses plus a radius from a bend, or they distort.

Common questions

What is a K-factor?

The ratio of the neutral axis position (measured from the inside of the bend) to the thickness. A K-factor of 0.33 means the neutral axis is a third of the way through the material.

What is the difference between bend allowance and bend deduction?

Bend allowance is the length of the arc of the bend. Bend deduction is the amount to subtract from the sum of the outside flange lengths to get the flat length.

How do I choose the die opening?

Six to eight times the thickness for steel up to 6 mm, ten to twelve times for thicker plate. A wider die lowers the force and gives a larger radius.

Sources

  • Machinery’s Handbook, Industrial Press (bend allowance and bend deduction); Kalpakjian, S. and Schmid, S., Manufacturing Engineering and Technology, Chapter 16 (bending).
  • Press-brake manufacturers’ tonnage charts (for the 1.33 UTS L T² / V relation); ASTM A653, EN 10130 (sheet).

Last reviewed: November 2, 2026