Press brake bend allowance and K-factor measurement setup

Press Brake Bend Allowance, K-Factor & Bend Deduction Guide

Press brake bend allowance determines how much material belongs inside a bend when a formed sheet-metal part is unfolded. The related K-factor describes the neutral-axis location, while bend deduction converts outside finished dimensions into a flat blank. These values are connected, but they are not interchangeable.

Quick answer: for a bend angle measured from flat, bend allowance is BA = A × (R + K × T), where A is the bend angle in radians, R is finished inside radius, K is K-factor and T is measured material thickness. Treat any generic K-factor as a planning value. Production accuracy comes from a test bend using the actual material, grain direction, punch, V opening and forming method.
Press brake bend allowance and K-factor measurement setup
Flat-pattern accuracy starts with the finished bend geometry and a measured result from the real press-brake setup.
Bend allowanceBA = A × (R + K × T)

Arc length through the bend along the neutral axis.

Outside setbackOSSB = tan(A ÷ 2) × (R + T)

Distance from tangent point to the theoretical outside sharp.

Bend deductionBD = 2 × OSSB − BA

Amount removed from the sum of two outside flange dimensions.

What Bend Allowance, K-Factor and Bend Deduction Mean

Term What it represents How it is normally used
Material thickness (T) Actual measured sheet thickness, not only the nominal gauge label. Radius, allowance, setback, tooling and tonnage calculations.
Inside radius (R) The finished radius on the inside surface of the formed bend. Geometry input. For air bending, the achieved radius depends strongly on the V opening and material.
Neutral axis A layer inside the bend zone with approximately no change in length. Its arc length becomes the bend allowance.
K-factor (K) Neutral-axis distance from the inside surface divided by thickness. A compact way for CAD and calculations to estimate flat development.
Bend allowance (BA) Developed arc length through the bend zone along the neutral axis. Add to inside tangent-to-tangent straight lengths.
Bend deduction (BD) Difference between twice the outside setback and the bend allowance. Subtract from the sum of finished outside flange dimensions.
Sheet metal neutral axis and flat-pattern development illustration
The outside of the bend stretches, the inside compresses and the neutral axis shifts toward the inside surface. Its position is represented by K × T.

How K-Factor Changes a Flat Pattern

K-factor is the neutral-axis offset divided by material thickness. A K-factor of 0.33 means the neutral axis is being modelled at 33% of the thickness from the inside surface. Autodesk and ANSYS both describe the same physical relationship: material inside the bend is compressed, material outside is stretched and the zero-strain layer lies between them.

One K-factor cannot describe every bend. The result changes with the radius-to-thickness relationship, material and temper, tooling, V opening, grain direction and whether the job is air bent, bottomed or coined. ANSYS specifically recommends reverse-calculating the actual K-factor from a formed sample when accuracy matters.

Do not copy a K-factor from an unrelated shop or CAD template and treat it as certified production data. It can be a useful starting point, but the bend table should ultimately belong to your material and tooling combination.

Illustration: sensitivity to K-factor

The table below holds thickness, radius and angle constant at 2.0 mm, 2.0 mm and 90°. It shows how only changing K-factor changes bend allowance and deduction.

K-factor Bend allowance Outside setback Bend deduction
0.30 4.084 mm 4.000 mm 3.916 mm
0.33 4.178 mm 4.000 mm 3.822 mm
0.38 4.335 mm 4.000 mm 3.665 mm
0.42 4.461 mm 4.000 mm 3.539 mm

Bend Allowance vs Bend Deduction: Which Method Should You Use?

Both methods can produce the same correct flat length. The difference is the dimensioning convention you start with.

  • Bend allowance method: add the straight inside tangent lengths and add BA for every bend.
  • Bend deduction method: add the finished outside flange dimensions and subtract BD for every bend.
  • CAD bend table: store measured allowance or deduction values for defined thickness, radius, angle, material and tooling conditions.

SOLIDWORKS documents the same distinction: flat length can be found by adding bend allowance to the tangent lengths or subtracting bend deduction from outside dimensions. The calculation method must match how the legs were measured.

Angle convention matters. In the formulas on this page, A is the angle the sheet is bent through from flat. A square 90° bend uses A = 90°, or π/2 radians. Some drawings and controls display the remaining included angle instead. Confirm the convention before calculating.

Metric Bend Allowance Example

2 mm sheet, 2 mm inside radius, 90° bend, K = 0.33

Inputs: T = 2.000 mm, R = 2.000 mm, A = 90° = 1.5708 rad, K = 0.33.

BA: 1.5708 × (2.000 + 0.33 × 2.000) = 4.178 mm.

OSSB: tan(45°) × (2.000 + 2.000) = 4.000 mm.

BD: 2 × 4.000 − 4.178 = 3.822 mm.

For outside legs of 50 mm and 40 mm, flat length = 50 + 40 − 3.822.

Planning flat length: 86.178 mm

Imperial Bend Deduction Example

0.060 in sheet, 0.060 in radius, 90° bend, K = 0.33

BA: 1.5708 × (0.060 + 0.33 × 0.060) = 0.1253 in.

OSSB: tan(45°) × (0.060 + 0.060) = 0.1200 in.

BD: 2 × 0.1200 − 0.1253 = 0.1147 in.

For outside legs of 2.000 in and 1.500 in, flat length = 2.000 + 1.500 − 0.1147.

Planning flat length: 3.3853 in

How to Build a Shop-Specific Bend Table

Define the real setup

Record material specification and temper, measured thickness, grain direction, punch tip radius, V opening, bend angle and forming method.

Cut a controlled test coupon

Use a known flat blank and keep the bend centred. The coupon should be large enough to measure both finished legs reliably.

Form using approved parameters

Confirm tooling and machine load ratings first. Use the same setup planned for production.

Measure the finished geometry

Measure both outside legs, the achieved angle and the actual inside radius after springback. Do not assume the punch tip equals the finished radius.

Calculate measured deduction

For one bend with outside dimensions, BD = outside leg A + outside leg B − original flat blank length.

Back-calculate allowance and K

BA = 2 × OSSB − BD. Then K = (BA ÷ A − R) ÷ T, using A in radians.

Repeat and store the result

Confirm with more than one coupon, then build a bend table by material, thickness, radius, V opening and angle. Autodesk notes that measured bend tables can better represent nonlinear equipment behaviour than one uniform K-factor.

Technician measuring the achieved inside radius of a press brake bend
Measure the achieved radius and angle after forming; springback and the real V-die geometry affect the bend table.

Common Flat-Pattern Errors

  • Using nominal gauge instead of measured thickness. Thickness affects BA, setback, natural radius and tonnage.
  • Assuming the punch radius becomes the inside radius. During air bending, the material and V opening strongly influence the achieved radius.
  • Mixing inside and outside dimensions. BA and BD workflows use different dimension references.
  • Using the included angle in a formula expecting bend angle. A 90° bend is simple; acute and obtuse bends make this mistake easier.
  • Ignoring grain direction and material lot variation. Both can move the measured result.
  • Applying one value to every tool and material. Build separate records for repeat production conditions.
  • Skipping machine and tooling checks. A correct flat pattern does not prove the setup is within tonnage, linear-load or sectional-load limits.

Continue the Press Brake Learning Path

Flat-pattern development works best when radius, V opening and bending force are considered together.

Bend Radius & Springback Guide V-Die Opening Guide Tonnage Charts by Material Interactive Tonnage Calculator Complete Tooling Selection Guide Education & Product Guides

Press Brake Tooling to Compare

Tooling selection affects the achieved radius and therefore the bend table. Confirm clamping style, angle, radius, opening, length and maximum linear load before ordering.

Amada style 60 degree two-V press brake die

2017 Two-V Die, 60°

Amada-style die with 16 mm and 20 mm openings and a listed 60 T/m maximum.

From $241 CAD

View Two-V Die
Amada style 45 degree press brake V die with 40 millimeter opening

2081 Single-V Die, 45°

Amada-style die with a listed 40 mm V opening and 100 T/m maximum.

From $580 CAD

View 40 mm V Die
Amada Promecam style 88 degree straight press brake punch

1011 Straight Punch, 88°

Amada/Promecam-style punch with a listed 0.8 mm tip radius and 100 T/m maximum.

From $202 CAD

View 88° Punch
Need a tooling and bend-development review?
Send the machine and holder model, material specification, measured thickness, bend length, V opening, target angle, finished dimensions and drawing.
Request a Tooling Review or Quote

Press Brake Bend Allowance FAQ

What is the difference between K-factor and bend allowance?

K-factor describes the neutral-axis position as a fraction of thickness. Bend allowance is the developed arc length calculated using that position, the inside radius and bend angle.

Is bend deduction the same as bend allowance?

No. Bend allowance is added to inside tangent lengths. Bend deduction is subtracted from the sum of outside flange dimensions. They are connected through outside setback.

What K-factor should I use for mild steel?

Use your validated shop bend table whenever possible. A generic value can help with an initial test blank, but the actual result depends on radius-to-thickness ratio, tooling, V opening, material condition and forming method.

Does K-factor change with V-die opening?

It can. In air bending, the V opening affects the achieved inside radius and deformation pattern. That changes the allowance or deduction measured from the formed coupon.

Can one bend deduction be used for every angle?

No. Angle is part of both the bend allowance and outside-setback equations. Record multiple angles when the shop produces more than one bend condition.

Should the customer or fabricator create the final flat pattern?

The fabricator usually has the best data for the actual material and tooling. When tight tolerances matter, coordinate the supplied model, drawing dimensions and bend-table responsibility before cutting production blanks.

Technical References

Next step: verify the achieved radius with the bend radius and springback guide, then confirm force using the press brake tonnage calculator.

Back to blog