FREE TOOL
Bend Allowance and Bend Deduction Calculator
Calculate sheet-metal bend allowance, outside setback and bend deduction from material thickness, inside bend radius, bend angle and K-factor. Add the two outside flange dimensions to get the flat blank length.
Bend allowance and bend deduction calculator
Assumes constant thickness through the bend. Confirm the K-factor with a test bend.
| Step | Formula | Value |
|---|---|---|
| Bend angle in radians | θ = 90° × π / 180 | 1.57080 rad |
| Bend allowance | BA = θ × (R + K × T) = 1.57080 × (3 + 0.33 × 2) | 5.749 mm |
| Outside setback | OSSB = tan(θ / 2) × (R + T) = tan(0.78540) × (3 + 2) | 5.000 mm |
| Bend deduction | BD = 2 × OSSB − BA = 2 × 5.000 − 5.749 | 4.251 mm |
| Flat blank length | L = A + B − BD = 50 + 30 − 4.251 | 75.749 mm |
Formulas used
- Bend angle in radians
- θ = A × π / 180
- Bend allowance
- BA = θ × (R + K × T)
- Outside setback
- OSSB = tan(θ / 2) × (R + T)
- Bend deduction
- BD = 2 × OSSB − BA
- Flat blank length (one bend)
- L = A_out + B_out − BD
Assumptions and limits
- A is the bend angle: the angle the flange is bent through (90° for an L bracket). If the drawing gives the included angle between flanges, use 180° minus that angle.
- R is the inside bend radius and T the material thickness, in the same unit.
- K is the neutral-axis position as a fraction of thickness, from 0 (inside surface) to 0.5 (mid-plane). It depends on material, tooling, radius-to-thickness ratio and process, so take it from your own test bends or your press brake supplier.
- Flange dimensions are measured to the outside mold line (the virtual sharp), which is how most drawings dimension formed parts.
- Thickness is assumed constant through the bend. Stretching, springback and coining are not modelled.
Worked example
Example: a 2 mm bracket with a 3 mm inside radius is bent 90°. Test bends in the shop gave a K-factor of 0.33. The outside flange dimensions are 50 mm and 30 mm. What is the flat blank length?
| Step | Formula | Value |
|---|---|---|
| Bend angle in radians | θ = 90° × π / 180 | 1.57080 rad |
| Bend allowance | BA = θ × (R + K × T) = 1.57080 × (3 + 0.33 × 2) | 5.749 mm |
| Outside setback | OSSB = tan(θ / 2) × (R + T) = tan(0.78540) × (3 + 2) | 5.000 mm |
| Bend deduction | BD = 2 × OSSB − BA = 2 × 5.000 − 5.749 | 4.251 mm |
| Flat blank length | L = A + B − BD = 50 + 30 − 4.251 | 75.749 mm |
Result: Bend allowance 5.749 mm, bend deduction 4.251 mm, so the flat blank is 75.749 mm long.
How to use bend allowance and bend deduction
Bend allowance vs bend deduction
Bend allowance is the length of the neutral axis through the bend. You add it to the straight flat lengths of each flange. Bend deduction is what you subtract from the sum of the outside flange dimensions. Both give the same flat length; use the one that matches how your part is dimensioned.
Most drawings dimension flanges to the outside mold line, so bend deduction is usually the faster route: add the outside dimensions and subtract one BD per bend.
Getting a K-factor you can trust
The K-factor is the biggest source of error. Bend a strip of known length in your own tooling, measure the outside flanges, and solve the bend deduction formula backwards for K. Record the material, thickness, die opening and punch radius with the result, because K changes with each of them.
Several bends
For a part with several bends, subtract one bend deduction per bend from the sum of all outside flange dimensions. Bends with different angles or radii each need their own BD.
Check the blank before cutting a batch
Cut and form one blank, measure the flanges, and adjust the K-factor if needed. Put the confirmed K-factor and blank length in the work instruction so every shift cuts the same blank.
Common mistakes
- Using the included angle as the bend angle. A 120° included angle is a 60° bend. Mixing the two gives a very wrong bend allowance.
- Copying a K-factor from a generic table. K depends on your material, tooling and radius. Confirm it with a test bend.
- Mixing inside and outside dimensions. Bend deduction assumes outside mold-line dimensions. Inside dimensions need a different setback.
- Applying one bend deduction to a part with several bends. Subtract one BD for every bend in the part.
- Ignoring the minimum flange length. A flange shorter than the outside setback cannot be formed as dimensioned. The calculator flags it.
Frequently asked questions
What is the bend allowance formula?
BA = θ × (R + K × T), where θ is the bend angle in radians, R the inside radius, K the K-factor and T the thickness. It is the arc length of the neutral axis through the bend.
What is the difference between bend allowance and bend deduction?
Bend allowance is added to the flat flange lengths. Bend deduction is subtracted from the outside flange dimensions. BD = 2 × OSSB − BA, so both give the same flat length.
What K-factor should I use?
K lies between 0 and 0.5 and depends on material, thickness, radius and tooling. The reliable way to get it is from a test bend in your own press brake. Your CAD system or tooling supplier may also publish values for their setups.
Does this work in inches?
Yes. Switch the unit to inches. All lengths must be in the same unit; the angle is always in degrees.
How do I calculate the flat length for a U channel?
Add the three outside dimensions and subtract one bend deduction for each of the two bends. If both bends share the same angle, radius and K-factor, subtract 2 × BD.
Sources
- Machinery's Handbook, Industrial Press — sheet-metal bending: allowance for bends from the neutral axis.
- Kalpakjian, S. and Schmid, S. R., Manufacturing Engineering and Technology, Pearson — sheet-metal bending, bend allowance and the neutral axis.
- Dassault Systèmes, SOLIDWORKS Help: K-Factor, Bend Allowance, Bend Deduction — definitions of BA, outside setback and BD.
Results are computed in your browser from the published formulas named above. They are an engineering aid, not a substitute for the governing standard, your drawing, or your customer's requirements.