How long is the flat blank for your bend?

What the number means

When sheet metal is bent, the outside of the bend stretches and the inside is squeezed, and somewhere between them lies a layer, the neutral line, whose length does not change. The flat blank you cut has to be as long as the legs plus the length of that line around the bend. That length is the bend allowance. Cut the blank too short and the finished part comes out small; cut it too long and the flange is oversize. The calculator also gives the bend deduction and the outside setback, the two numbers shops use when the drawing is dimensioned to the outside corners, and the flat length of an L or U part.

The formulas

With the sheet turned through angle θ, inside radius R, thickness T and K-factor K: BA = θ × (π/180) × (R + K × T), with θ in degrees. R + K·T is the radius of the neutral line. The outside setback is OSSB = tan(θ/2) × (R + T), the distance from where the bend starts to the sharp corner. The bend deduction is BD = 2 × OSSB − BA, and the flat length is the sum of the outside leg dimensions minus one BD for each bend. The setback is the same multiplication the FAA teaches for aircraft sheet metal: setback = K × (bend radius + metal thickness), where its K-chart is simply tan(θ/2).

Worked example

A bracket from 0.064-inch sheet, inside radius 0.125 inch, bent 90° by air bending in a medium material. The radius is 1.95 times the thickness, so the table gives K = 0.43. The neutral line has a radius of 0.125 + 0.43 × 0.064 = 0.1525 inch, and the allowance is (π/2) × 0.1525 = 0.240 inch. The outside setback is tan 45° × (0.125 + 0.064) = 0.189 inch, so BD = 2 × 0.189 − 0.240 = 0.138 inch. For outside legs of 2 and 1.5 inches the flat length is 3.5 − 0.138 = 3.362 inch. The FAA's own example, a 0.064-inch sheet bent 45° over a 0.25-inch radius, gives a setback of 0.41421 × (0.25 + 0.064) = 0.130 inch.

Rule-of-thumb K-factors

The table gives K for the three common ways of forming (air bending, bottoming, coining), soft / medium / hard material, and the radius as a multiple of the thickness. It comes from a general manufacturing reference and is only a starting point.

Limits of this method

The formula assumes the neutral line sits at a fixed fraction of the thickness. It does not: it moves toward the inside as the radius gets smaller relative to the sheet, as springback, tooling and the grain direction change, and the sources that publish K-factor tables say the real values can differ a lot from the table. For parts with tight tolerances, make a test bend, measure the flat and the finished leg, and solve for your own K. Also keep inside the minimum radius for the alloy and temper: Table 4-6 of the FAA circular lists recommended radii for aluminum as multiples of the thickness, and bending tighter can crack the outside surface. Finally, the results are for a single sharp-cornered bend with an unchanged thickness; joggles, hems and bends close to a hole or a previous bend need their own allowances.

What is bend allowance?

Bend allowance is the length of the arc that the bend takes in the flat pattern, measured along the neutral line, the layer of the sheet that is neither stretched nor squeezed. For a 0.064-inch sheet bent 90° over an inside radius of 0.125 inch with K = 0.43, it is 0.240 inch. Add the straight parts of the two legs and this arc, and you have the length of the blank you have to cut.

What is the K-factor and what value should I use?

The K-factor is the distance of the neutral line from the inside face, as a fraction of the thickness: 0 would be the inside surface, 0.5 the middle of the sheet. It usually lands between 0.3 and 0.5 and gets bigger as the radius grows. The rule-of-thumb table on this page runs from 0.33 (air bending of soft material with a radius up to the thickness) to 0.50 (any radius over three thicknesses). It is a starting point only: the safe way is to bend a test strip on your own press brake and back out K from the measured flat length.

What is the difference between bend allowance, bend deduction and setback?

Bend allowance is the arc length. The outside setback is the distance from the tangent line where the bend begins to the virtual sharp corner (the mold line): tan(θ/2) × (R + T), which is 0.130 inch for the FAA's 45° example with a 0.25 inch radius. Bend deduction is what you subtract from the sum of the outside leg dimensions to get the flat length: BD = 2 × setback − BA, 0.138 inch in the example above. If you dimension a part to the outside corners, use the deduction; if you dimension it to the tangent lines, add the allowance.

Is the radius the inside or the outside radius?

The inside radius. The FAA's Advisory Circular 43.13-1B says that in aviation sheet-metal work the term bend radius means the inside radius, and the calculator uses the same convention. If your drawing gives the outside radius, subtract the thickness first. The angle is how far the sheet is turned, so an L-shaped bracket is 90°; the FAA's example of a 135° closed angle is a 45° bend.

Can I bend a very tight radius?

Not always. The minimum radius depends on the alloy, the temper and the thickness; Table 4-6 of AC 43.13-1B lists recommended inside radii for 90° bends in aluminum alloys as multiples of the thickness t, from nothing for soft annealed sheet to several thicknesses for hard tempers such as 2024-T6 and 7075-T6. The same advisory circular asks for bend lines at an angle to the grain, preferably 90°, and for relief holes at the ends of bend lines. A tighter radius than the table recommends can crack the outside of the bend.

Does the angle change anything for flat-length math?

Yes, through both terms: the arc grows with the angle, and the setback follows tan(θ/2), which grows much faster as the bend approaches 180°. At 45° the setback factor is 0.4142, at 90° it is 1.000 and at 135° it is 2.414, the numbers of the FAA K-chart. Enter the angle the sheet is turned through, not the angle left between the flanges.

Sources: FAA Advisory Circular 43.13-1B, “Acceptable Methods, Techniques, and Practices — Aircraft Inspection and Repair” (9/8/98), paragraphs 4-55 and 4-56, Table 4-6 (recommended bend radii of aluminum alloys) and Table 4-7 (K-chart for setback, worked example 0.064-inch sheet, 45°, setback 0.130 inch); formulas for bend allowance and bend deduction and the K-factor range of 0.3 to 0.5 as given in Wikipedia, “Bending (metalworking)”; the rule-of-thumb K table is Wikipedia's summary of Todd, Allen and Alting, Manufacturing Processes Reference Guide (Industrial Press, 1994), which itself warns that actual results vary. Related: metal weight calculator, hole pattern calculator, right triangle calculator and decimal to fraction calculator. How we check our calculators.