Bend Allowance and K-Factor Calculator
Bend allowance is the length of the neutral axis through a bend: BA = angle in radians × (R + K × T). Enter thickness, inside radius, bend angle and K-factor below to get the bend allowance, bend deduction and flat length, or measure a test bend to find your K-factor.
Bend allowance, bend deduction and flat length
All lengths in one unit, millimetres or inches.
| Material thickness | ||
| Inside bend radius; 0 for a sharp bend | ||
| Angle bent through: 90 for an L-bracket | ||
| Starting values in the chart below | ||
| Outside dimension, to the mold line | ||
| Outside dimension, to the mold line |
| Bend allowance (BA) | 6.063 |
| Outside setback (OSSB) | 5.000 |
| Bend deduction (BD) | 3.937 |
| Flat length (L1 + L2 − BD) | 76.063 |
K-factor from a test bend
Bend a strip, measure it, and get the K-factor your brake actually gives.
| Material thickness | ||
| Inside bend radius; 0 for a sharp bend | ||
| Angle bent through: 90 for an L-bracket | ||
| Outside dimension after bending | ||
| Outside dimension after bending | ||
| Length of the strip before bending |
| K-factor | 0.429 |
| Use this K-factor for this material, thickness, radius and tooling. | |
What is bend allowance?
Bend allowance is the arc length of the neutral axis through the bend: the material the bend itself uses up. Add it to the two straight flanges, measured to where the bend starts, and you have the flat blank. It depends on thickness, inside radius, bend angle and K-factor.
The formula is BA = A × π / 180 × (R + K × T), where A is the bend angle in degrees, R the inside radius, T the thickness and K the K-factor. Only the neutral axis keeps its length when metal bends: the outside stretches and the inside compresses.
What is the K-factor in sheet metal?
The K-factor is where the neutral axis sits, as a fraction of the thickness measured from the inside of the bend. K = 0.5 puts it at mid-thickness; bending pulls it toward the inside, so real values fall between about 0.3 and 0.5. It is the one number in the formula you cannot read off a drawing.
It changes with the material, its hardness and grain, the radius-to-thickness ratio, and the tooling and method (air bending, bottoming or coining). That is why two shops can quote different flat lengths for the same part, and why a test bend beats any chart.
What K-factor should I use?
Start from the chart below for air bending, then confirm with a test bend. Pick the row by how the inside radius compares with the thickness, and the column by the material: soft for aluminium and copper, medium for mild steel, hard for stainless steel.
| Inside radius | Soft | Medium | Hard |
|---|---|---|---|
| Up to 1 x thickness | 0.33 | 0.38 | 0.40 |
| 1 to 3 x thickness | 0.40 | 0.43 | 0.45 |
| Over 3 x thickness | 0.50 | 0.50 | 0.50 |
These are common starting values, not a property of the material. A CAD program’s default K-factor is a placeholder too: change it to your shop’s number before you trust a flat pattern.
How do I find the K-factor from a test bend?
Cut a strip of the real material, measure its length, bend it once at a known angle with your tooling, then measure both flanges to the outside. Enter those numbers in the second calculator above. It works the bend deduction backwards to the bend allowance and solves for K.
- Cut a strip about 50 mm (2 in) wide and note its exact length: the flat blank.
- Bend it through 90 degrees with the punch and die you will use on the part.
- Measure each flange from its end to the outside mold line, where the two outside faces would meet.
- Measure the inside radius with a radius gauge, and the thickness with a micrometer.
Keep the K-factor with the material, thickness and tooling it came from. A different die opening gives a different inside radius in air bending, and so a different K.
What is the difference between bend allowance and bend deduction?
Bend allowance is added to flanges measured to the bend tangents; bend deduction is subtracted from flanges measured to the outside mold line. They describe the same blank: BD = 2 × OSSB − BA, where the outside setback OSSB = tan(A / 2) × (R + T).
Drawings usually dimension a formed part to the outside, so bend deduction is the quicker route to a flat length: add the outside dimensions and subtract one bend deduction per bend.
How do I calculate the flat length of a sheet metal part?
Add the outside dimensions of every flange, then subtract one bend deduction for each bend. For a single 90 degree bend in 2 mm material with a 3 mm inside radius, K 0.43, and flanges of 50 mm and 30 mm, the flat length is 50 + 30 − 3.94 = 76.06 mm.
| Step | Working | Result |
|---|---|---|
| Bend allowance | 1.5708 × (3 + 0.43 × 2) | 6.06 mm |
| Outside setback | tan 45° × (3 + 2) | 5.00 mm |
| Bend deduction | 2 × 5.00 − 6.06 | 3.94 mm |
| Flat length | 50 + 30 − 3.94 | 76.06 mm |
The calculator above opens with these numbers, so you can check it against the working before you use your own.
Frequently asked questions
What is the formula for bend allowance?
Bend allowance = bend angle in radians × (inside radius + K-factor × thickness). For a 90 degree bend in 2 mm material with a 3 mm inside radius and a K-factor of 0.43, that is 1.5708 × 3.86 = 6.06 mm.
What is a good K-factor for sheet metal?
For air bending, about 0.33 to 0.45 when the inside radius is up to three times the thickness, and 0.5 for larger radii. Softer materials and tighter radii sit at the low end. Measure a test bend for the exact number on your brake.
What is the difference between bend allowance and bend deduction?
Bend allowance is the length of material in the bend, added to the flat flanges. Bend deduction is what you subtract from the outside dimensions to get the flat length. Both describe the same blank; use whichever matches how the drawing is dimensioned.
Can the K-factor be more than 0.5?
Not in a real bend. The K-factor is where the neutral axis sits as a fraction of the thickness from the inside surface, and bending pushes it inward, so it falls between 0 and 0.5. A calculated value above 0.5 usually means a flange was measured to the wrong line.
Does the bend angle mean the angle between the flanges?
No. Use the angle the flange is bent through: 90 degrees for an L-bracket, 45 degrees for a flange bent up to 135 degrees from the sheet. The two are the same number only at 90 degrees.
Does it work in inches?
Yes. The calculator has no units of its own: enter thickness, radius and flanges all in inches, or all in millimetres, and every result comes out in the same unit. The angle is always in degrees and the K-factor has no unit.
Have a drawing of the part but no CAD model?
Upload the drawing to Drawing to STEP: a PDF, PNG or JPG up to 10 MB becomes a STEP model of the formed part in minutes, with files from $29.99. Open the STEP in your CAD program’s sheet-metal tool and unfold it with your K-factor.