Bend Allowance Calculator
Work out sheet metal bend allowance, bend deduction and flat length from thickness, inside radius, bend angle and K-factor. Also gives the outside setback, in inches or millimeters, and takes either the bend angle or the angle between the flanges.
Your numbers
Measured, not nominal gauge: gauges differ by material.
The radius on the inside of the bend; in air bending it follows the die opening.
A 90° part is 90 either way. A part bent to 120° between the flanges is a 60° bend.
Default 0.43: air bending, medium material, R between T and 3T (Diegel). See the K-factor table below, or use your shop's own.
Optional: each flange measured on the outside, from the edge to the corner (mold point), for the flat length.
Bend allowance (BA)
–
- Outside setback (OSSB)
- –
- Bend deduction (BD)
- –
- Flat length
- –
- Bend angle used
- –
- Rule-of-thumb K for this R/T (air bending)
- –
The K-factor sets the answer. Rules of thumb get close; a test bend on your own brake and tooling gets it right (bend a measured strip and back out K).
One bend at a time. For a part with several bends, subtract one bend deduction per bend.
The calculation runs in your browser and ParrotNotes does not store your numbers. They sit in the page address so you can bookmark or share the result.
How bend allowance is worked out
Bending stretches the outside of the sheet and compresses the inside. Somewhere between the two is the neutral axis, a line that keeps its length. The bend allowance is the length of that line through the bend: an arc of radius R + K × T over the bend angle, so BA = π/180 × A × (R + K × T).
The FAA's Aviation Maintenance Technician Handbook writes the same idea with fixed constants, BA = (0.01743 × R + 0.0078 × T) × N, which puts the neutral axis at about 0.445 of the thickness. Its example, 90° with R = 0.16 in in 0.040 in sheet, comes to 0.279 in; with K at half the thickness, its other example, R = 0.250 in in 0.051 in sheet, comes to 0.4327 in.
Outside setback and bend deduction
The outside setback is the distance from where the bend starts to the corner the two outside faces would make if the bend were sharp (the mold point): OSSB = tan(A/2) × (R + T). At 90°, tan 45° is 1 and the setback is simply R + T; the FAA's 0.16 in radius in 0.040 in sheet has a setback of 0.2 in.
Drawings usually dimension flanges to the outside corner. Two flanges each measured that way count the corner twice and miss the curve, so you subtract the bend deduction: BD = 2 × OSSB − BA. Diegel's BendWorks notes give the same relation the other way round, BA = 2 × OSSB − BD.
Flat length for a part
With the flanges measured on the outside to the corner, the flat length is flange 1 + flange 2 − BD. With the flat legs measured to the bend tangent lines instead, it is leg 1 + leg 2 + BA. Both give the same blank.
For a part with several bends, subtract one bend deduction per bend. The FAA's U-channel (1 + 2 + 1 in outside, two 90° bends, R 0.16 in, T 0.040 in) is 4 − 2 × 0.121 = 3.76 in of flat with the exact formula; the handbook, with BA rounded to 0.27, gets 3.74 in.
Choosing a K-factor
The K-factor is the neutral axis position divided by the thickness. It depends on the material, the radius against the thickness, and how the part is bent: air bending, bottoming or coining. Diegel's BendWorks notes give the rules of thumb in the table below; the calculator opens on 0.43 (air bending, medium material, R between T and 3T) and shows the air bending range for your R/T under the result.
The way to pin K down is a test bend: bend a measured strip on the brake and tooling you will use, measure both flanges, and work back: BD = flange 1 + flange 2 − strip length, BA = 2 × OSSB − BD, K = (BA ÷ (π/180 × A) − R) ÷ T. That K then fits your shop's radius and tooling.
K-factor rules of thumb
From Olaf Diegel's BendWorks notes (2002). Starting values for non-precision work; a test bend on your own tooling beats them.
| Method | Inside radius | Soft | Medium | Hard |
|---|---|---|---|---|
| Air bending | 0 to T | 0.33 | 0.38 | 0.4 |
| Air bending | T to 3T | 0.4 | 0.43 | 0.45 |
| Air bending | Over 3T | 0.5 | 0.5 | 0.5 |
| Bottoming | 0 to T | 0.42 | 0.44 | 0.46 |
| Bottoming | T to 3T | 0.46 | 0.47 | 0.48 |
| Bottoming | Over 3T | 0.5 | 0.5 | 0.5 |
| Coining | 0 to T | 0.38 | 0.41 | 0.44 |
| Coining | T to 3T | 0.44 | 0.46 | 0.47 |
| Coining | Over 3T | 0.5 | 0.5 | 0.5 |
For sheet metal sales and sales engineers
A bent part is quoted from the RFQ call as much as from the drawing: the flange lengths the buyer needs, the material and gauge, which side the dimensions are to, the tolerance, the quantity. Get one of them wrong and the first article comes back.
Sources, each read on 2026-10-28. Results are for one bend; your shop's bend tables or test bends decide the final blank:
More for manufacturers' reps and sales engineers: Sales engineer, What is an RFQ, RFQ template, Manufacturers' rep.
The part comes in on the RFQ call
Flange lengths, material, gauge, which side the dimensions are to and the tolerance are all said on the call before the drawing arrives. Record it in ParrotNotes and get a transcript, a summary and the action items, so the quote matches what the buyer asked for.
Get Started FreeRelated tools
- Steel Weight CalculatorWeigh steel, stainless, aluminum and other metals as plate, sheet, bar, tube, pipe or angle, per foot or meter, per piece and for the order.Open the tool
- Torque Conversion CalculatorConvert torque between newton meters, foot-pounds, inch-pounds, kilogram-force meters and more, with a quick chart for common values.Open the tool
- Feeds and Speeds CalculatorWork out spindle rpm, feed rate and material removal rate for milling, drilling and turning from the cutting speed, diameter, teeth and chip load.Open the tool
- Lead Time CalculatorCount business days from order to delivery, find the order-by date for a needed date, and add up supplier, production and shipping lead times.Open the tool