How to work out the flat length of a bent part

How long a blank does a bent part need? The answer depends on where the flanges are measured to and on how much material the bend itself uses. Here are the two standard ways to work it out — straight legs plus bend allowance, or outside dimensions minus bend deduction — on one worked example, with the trap that catches most people: the bend angle.

Published 2026-10-30. Rather have the numbers worked out? Single Bend Flat Pattern Configurator does it in your browser.

What you are making

The worked example: an angle bent from 2 mm sheet with a 2 mm inside radius, flanges of 50 and 30 measured to the outside, bent to a square corner. The K-factor — where the neutral layer sits in the thickness — is taken as 0.44; for your own number, see the K-factor tool.

Figure 1. The formed part, drawn by the single-bend tool's code.

1. Know what the flanges are measured to

A drawing may dimension a flange to the mold line — where the flat outside faces would meet if extended past the bend: the FAA calls it an extension of the flat side beyond the radius (FAA-H-8083-31B, p. 4-59). The bend itself starts at the tangent line, where the flat stops and the radius begins. The distance between the two along the flange is the outside setback: (inside radius + thickness) × tan(angle ÷ 2), which for a square bend is simply R + T (FAA, p. 4-59; Benson). Here: (2 + 2) × tan 45° = 4.000.

2. Way one: straight legs plus bend allowance

Take the setback off each outside flange to get the straight legs: 50 − 4 = 46.00 and 30 − 4 = 26.00. The bend uses the length of the neutral layer through it, the bend allowance: angle in radians × (inside radius + K × thickness), or π × (R + K·T) × A ÷ 180 with A in degrees (SOLIDWORKS help, “K-Factor”). Here π/2 × (2 + 0.44 × 2) = 4.524. The blank is the two legs plus the allowance: 46.00 + 26.00 + 4.524 = 76.524.

3. Way two: outside dimensions minus bend deduction

Shops that work from outside dimensions add the flanges and subtract a bend deduction per bend: twice the outside setback less the bend allowance (Benson; SOLIDWORKS help, “Bend Allowance and Bend Deduction”). Here 2 × 4 − 4.524 = 3.476, and 50 + 30 − 3.476 = 76.524 — the same blank, because it is the same arithmetic rearranged.

Figure 2. The blank, 76.524 long. The bend zone runs from 46.00 to 50.52 from the left end; its middle, 48.262, is where the single-bend tool puts the bend line.

4. The trap: which angle?

Every formula above uses the angle the sheet is bent through — 90° for a square corner, 0° for flat stock. A drawing that shows the included angle between the flanges has to be converted: bend angle = 180° − included angle (FAA, p. 4-66). At 90° the two readings agree, which is why the mistake survives. At an included angle of 45° the part is bent through 135°: the blank is 67.47. Read the 45 as the bend angle instead and you get 78.95 — 11.48 too long.

5. More than one bend

Every bend contributes its own allowance (or deduction); the legs between two bends lose a setback at each end. The profile builder does this for open profiles with any number of bends, and the bend deduction chart tabulates the values for your thickness and K.

Common mistakes

Mixing datums: outside flanges with an allowance, or tangent legs with a deduction.
Using the included angle as the bend angle.
Using a K-factor from a table for a radius, material or tool it was not measured for.
Using the punch radius as the inside radius of an air bend — measure the part.

How this matches the tool

The single-bend tool asks which datum the flanges are measured to, converts everything to straight legs first and applies one formula, and exports the blank as DXF with the bend line on its own layer. Every number on this page was produced by its own code when the page was built.

Sources

Skip the arithmetic

Single Bend Flat Pattern Configurator — Flat length and bend line from your finished flanges — with an explicit datum, a formed section you can check against, and a DXF blank.

Free, in your browser; nothing you type is sent anywhere. How the tools are checked is on the Verification page. Rather have the part drawn for you? Drafting for small shops, quoted per job.