Quiénes somos
Durmapress specializes in designing, manufacturing, and selling various metal processing equipment, including bending machines, shears, punches, and laser cutting machines. The company was founded in 2014, with years of experience and technology accumulation. DurmaPress has become one of the well-known brands in China's metal processing machinery industry.
Póngase en contacto con nosotros
Entradas recientes
Categorías
Síguenos
Nuevo vídeo semanal
Table of Contents
Bend deduction is the length you subtract from the sum of a part's outside flange dimensions to get the correct flat blank size before bending. The core bend deduction formula is:
BD = 2 × OSSB − BA
You need it because sheet metal stretches when it bends. If you cut a blank equal to the finished outside dimensions, the part comes out too long. The bend deduction corrects for that stretch, so your flat pattern produces accurate flange lengths and correctly located bend lines after forming.
This guide explains the bend deduction formula for press brake bending, including calculation steps, flat pattern examples, and the practical factors that affect real-world results. Because we build press brakes, it also covers how the number on paper behaves on an actual machine.
Bend Deduction Formula—Quick Answer
Standard formula — use this when you already have your bend allowance and outside setback:
BD = 2 × OSSB − BA
Formula with input parameters — use this to calculate directly from material and tooling values:
BD = 2 × (R + T) × tan(A / 2) − BA
where BA = (π / 180) × A × (R + K × T)
Then find your flat pattern length:
Single bend: Flat Length = L1 + L2 − BD
Multiple bends: Flat Length = Σ outside dimensions − Σ bend deductions
L1 and L2 are the finished outside dimensions, measured to the theoretical sharp corner (the outside mold line / apex).
Variable Definitions
| Symbol | Nombre | What it is |
|---|---|---|
| BD | Bend Deduction | Length removed from the outside dimension total to get the flat length |
| BA | Bend Allowance | Arc length of the bend measured along the neutral axis |
| OSSB | Outside Setback | Distance from the theoretical sharp corner to the tangent point of the bend |
| R | Inside Bend Radius | The radius formed on the inside of the bend |
| T | Material Thickness | Actual decimal thickness of the sheet |
| A | Bend Angle | The angle the material is bent through (see angle note below) |
| K | K-Factor | Ratio that locates the neutral axis inside the material thickness |
Keep three to four decimal places through the calculation and round only the final result. Small rounding errors grow quickly on multi-bend parts.
How to Calculate Bend Deduction Step by Step
The workflow is always the same: parameters → bend allowance → outside setback → bend deduction → flat pattern.
Step 1 — Confirm Your Inputs
Before you touch the formula, lock down five values that reflect the actual job, not textbook defaults:
- Material and thickness (
T) — use the real decimal thickness, not just the gauge number. - Inside radius (
R) — the radius the tooling actually produces, not an assumed value. - Bend angle (
A) — confirm which angle convention your formula uses (explained in the next section). - K-factor (
K) — a validated value for that material and tooling. - Bending method — air bending, bottoming, or coining, because it changes the radius.
Step 2 — Calculate Bend Allowance
BA = (π / 180) × A × (R + K × T)
This formula applies when the bend angle A is defined as the angle of rotation from the flat state (explained in the next section). Bend allowance is the arc length of material consumed inside the bend. It is not the amount you subtract from the flange total—it is an input used inside the bend deduction formula. For a full treatment of neutral axis and K-factor selection, see our detailed bend allowance formula guide. To look up a validated K-factor for your material, see our K-Factor table.
Step 3 — Calculate Outside Setback
OSSB = (R + T) × tan(A / 2)
Every bend has two outside setbacks—one on each flange—which is why the bend deduction formula starts with 2 × OSSB. The setback is the geometric distance between the sharp theoretical corner (used on drawings) and the point where the flat metal begins to curve.
Step 4 — Calculate Bend Deduction
OSSB = (R + T) × tan(A / 2)
You are removing the double-counted sharp corner and replacing it with the real curved arc. What remains is the material you must deduct from the outside dimension total.
Step 5 — Calculate Flat Pattern Length
Subtract one bend deduction for each bend from the sum of the finished outside dimensions:
Flat Length = Σ outside dimensions − Σ bend deductions
When you lay out bend lines, each outer flange takes half a bend deduction, and a section sitting between two bends takes a full bend deduction (half from each side).
Bend Angle vs Included Angle: Which Angle Does the Formula Use?
This is the single most common source of wrong bend deduction values, so confirm it before you calculate.
- Included angle — the angle inside the finished part. A right-angle bracket has a 90° included angle.
- Bend angle (complementary / excluded angle) — how far the material is rotated from flat. A right-angle bracket is bent 90° from flat.
The formulas in this guide use the bend angle measured from flat. Convert an included angle like this:
Bend angle A = 180° − included angle
| Finished (included) angle | Bend angle from flat (`A`) |
|---|---|
| 90° | 90° |
| 120° | 60° |
| 135° | 45° |
A 90° bend is dangerous precisely because both numbers are 90°—a wrong convention produces the right answer, so the mistake stays hidden until you bend a non-90° part. Always check what your CAD software, calculator, or press brake control expects.
90-Degree Bend Deduction Formula Example
Let's calculate a real single-bend part in 5052 aluminum, air formed.
Inputs
| Parameter | Valor |
|---|---|
Material thickness T
|
0.080 in |
Inside radius R
|
0.050 in |
K-factor K
|
0.43 |
Bend angle A
|
90° |
| Finished base | 6.000 in |
| Finished flanges | 2.000 in each (two bends) |
Step 1 — Bend allowance
Subtract one bend deduction for each bend from the sum of the finished outside dimensions:
BA = (π / 180) × 90 × (0.050 + 0.43 × 0.080)
BA = 1.5708 × (0.050 + 0.0344)
BA = 1.5708 × 0.0844
BA = 0.1326 in
Step 2 — Outside setback
OSSB = (0.050 + 0.080) × tan(90 / 2)
OSSB = 0.130 × tan(45°)
OSSB = 0.130 × 1
OSSB = 0.1300 in
Step 3 — Bend deduction
BD = 2 × 0.1300 − 0.1326
BD = 0.2600 − 0.1326
BD = 0.1274 in
Step 4 — Flat pattern length
Subtract one bend deduction for each bend from the sum of the finished outside dimensions:
Flat Length = 2.000 + 6.000 + 2.000 − (2 × 0.1274)
Flat Length = 10.000 − 0.2548
Flat Length = 9.7452 in
Bend line placement
| Section | Finished Outside | Flat Dimension |
|---|---|---|
| Left flange | 2.000 in | 1.9363 in |
| Base | 6.000 in | 5.8726 in |
| Right flange | 2.000 in | 1.9363 in |
| Total | 10.000 in | 9.7452 in |
Each flange loses half a bend deduction (0.0637 in), and the base—sitting between two bends—loses a full bend deduction (0.1274 in). Cut the blank at 9.7452 in with bend lines at those positions, and the formed part measures 6.000 in with two 2.000 in flanges.
For users working in metric units, the same calculation applies—simply enter thickness, radius, and dimensions in millimeters. The formula and workflow do not change.
Multi-Bend Flat Pattern Calculation
On production parts, bend deductions add up—and so do errors. Here is a top-hat channel in 16-gauge (0.060 in) cold-rolled steel, air formed, with four identical 90° bends.
Inputs
| Parameter | Valor |
|---|---|
Material thickness T
|
0.060 in |
Inside radius R
|
0.075 in |
K-factor K
|
0.42 |
Bend angle A
|
90° |
Bend deduction per bend
BA = 1.5708 × (0.075 + 0.42 × 0.060) = 1.5708 × 0.1002 = 0.1574 in
OSSB = (0.075 + 0.060) × tan(45°) = 0.135 in
BD = 2 × 0.135 − 0.1574 = 0.1126 in
Outside dimensions (five sections, four bends)
| Section | Outside Dimension |
|---|---|
| Left flange | 0.750 in |
| Left wall | 1.000 in |
| Top | 2.000 in |
| Right wall | 1.000 in |
| Right flange | 0.750 in |
| Sum | 5.500 in |
Flat pattern length
Flat Length = 5.500 − (4 × 0.1126)
Flat Length = 5.500 − 0.4504
Flat Length = 5.0496 in
How Errors Accumulate
Suppose a designer pulls a generic 0.100 in bend deduction from an old chart instead of the correct 0.1126 in. The per-bend error is only 0.0126 in—seemingly harmless.
Wrong flat length = 5.500 − (4 × 0.100) = 5.100 in
Correct flat length = 5.0496 in
Total error = 0.0504 in
That 0.050 in stacks up across four bends, and the finished part comes out oversized with mounting holes that no longer line up with the mating assembly. The rule: one correct bend deduction per bend combination. Bends with different angles, radii, or tooling each need their own value.
Bend Deduction Chart (90° Air Bend, Reference Values)
A bend deduction chart or bend deduction table speeds up flat pattern work by giving you a starting value at a glance. The chart below shows approximate 90° bend deductions for common materials. Treat it as a reference only—verify against your own tooling for tight-tolerance parts.
| Espesor | Inside Radius | Ángulo | K-Factor | Approx. BD |
|---|---|---|---|---|
| 0.048 in (18 ga) | 0.060 in | 90° | 0.42 | ~0.090 in |
| 0.060 in (16 ga) | 0.075 in | 90° | 0.42 | ~0.113 in |
| 0.075 in (14 ga) | 0.090 in | 90° | 0.42 | ~0.138 in |
| 0.080 in (5052 Al) | 0.050 in | 90° | 0.43 | ~0.127 in |
| 0.105 in (12 ga) | 0.120 in | 90° | 0.42 | ~0.190 in |
Values assume air bending and consistent tooling. Because inside radius depends on the actual V-die and material, use these figures for estimating, then confirm with a test bend for production.
Bend Allowance vs Bend Deduction
Both describe how metal stretches in a bend, but they answer different questions and are measured from different reference points.
| Bend Allowance (BA) | Bend Deduction (BD) |
|---|---|
| Arc length along the neutral axis | Amount removed from outside dimension total |
| Neutral axis (inside the metal) | Outside mold line (what your calipers read) |
| Adds the bend arc between flat flanges | Subtracts from summed outside flanges |
Flat = flanges + BA
|
Flat = outside sum − BD
|
Both give the same flat length when the inputs and dimensioning convention are consistent. Most fabrication shops prefer bend deduction because it references the outside mold line—the surface you actually measure with calipers.
For a full breakdown of when to use each, see our dedicated Bend Allowance vs Bend Deduction article.
How Press Brake Tooling Affects Bend Deduction
The formula assumes a fixed inside radius. On a real press brake, the tooling largely sets that radius—so the tooling quietly controls your bend deduction. For deeper detail, see our guides on utillaje para prensas plegadoras and the V-die opening chart.
V-Die Opening and Inside Radius
In air bending, the part does not wrap the punch tip. Instead, the inside radius forms as a percentage of the V-die opening. As a general guideline, many shops use approximate radius-to-opening relationships that vary by material, but the actual inside radius should always be verified from the formed part. Change the die, and you change the radius.
In practice, a wider V-die tends to produce a larger inside radius. Because a larger radius increases bend allowance and shifts the setback, your bend deduction changes too. Calculate BD with the radius the die actually produces, not a nominal number.
Inside Radius Drives the Whole Calculation
Radius appears in both BA y OSSB, so it has an outsized effect on bend deduction:
| Inside Radius (0.060 in CRS, 90°, K=0.42) | Approx. BD |
|---|---|
| 0.060 in | ~0.106 in |
| 0.075 in | ~0.113 in |
| 0.093 in | ~0.120 in |
A radius change of a few thousandths meaningfully moves your flat pattern.
Air Bending vs Bottoming
- Air bending — the punch stops short of the die bottom; the radius depends on the die opening. Flexible, lower tonnage, but the radius must be verified.
- Bottoming — the punch presses the material to the die bottom; the punch and die more directly control the radius, giving more repeatable results at higher tonnage.
The two methods can produce different radii—and therefore different bend deductions—from the same material. If your test bend was bottomed but the production run is air formed, your calculated BD will be wrong.
Why Theoretical Bend Deduction Differs from Actual Results
A perfect calculation can still produce a bad part. The formula is only as good as its inputs and the consistency of the process.
- Material thickness variation — a skid measuring 0.004 in over nominal shifts both BA and OSSB. Always use the actual decimal thickness.
- Material and lot differences — alloy, temper, coating, and even mill run change how a sheet stretches. A new lot can move your K-factor.
- Actual vs assumed radius — worn tooling and a changed die opening alter the formed radius, and radius drives everything.
- Springback — the metal relaxes when the ram retracts, so the achieved angle differs from the commanded angle. If the operator over-bends to hit the target, the effective geometry—and the deduction—shifts.
- Grain direction — bending across versus along the grain changes the radius and tonnage slightly, which nudges the result.
Treat the formula as a strong starting point, then confirm it against the real setup for tight-tolerance work.
How to Correct Bend Deduction and Avoid Common Errors
The most reliable bend deduction is one you measure, not one you assume. The quickest way to get an accurate value—and avoid the mistakes below—is a test bend.
Verify with a test bend:
- Shear a coupon from the production lot to a known flat length (for example, 4.000 in).
- Bend a centered 90° using the same material, punch, V-die, and method as the run.
- Measure both outside flanges to the apex, then reverse calculate:
BD (actual) = (Flange 1 + Flange 2) − Original flat length
Example: (2.065 + 2.065) − 4.000 = 0.130 in
4. Update your CAD or bend tables with the measured value, then confirm a first-article part before running the batch.
Common calculation errors to check for:
| Mistake | Fix |
|---|---|
| Confusing BA with BD | BA is arc length; BD is what you subtract from outside dimensions |
| Wrong bend angle |
Convert: A = 180° − included angle
|
| Wrong inside radius | Use the radius the die actually produces |
| Wrong material thickness | Measure and use actual decimal thickness |
| Ignoring tooling conditions | Account for V-die opening, wear, and bending method |
| One BD for every bend | Each angle/radius/tooling combination gets its own BD |
Keep full decimal precision until the end, keep inch and metric values separate, and never subtract a bend deduction twice for the same bend.
PREGUNTAS FRECUENTES
The standard form is BD = 2 × OSSB − BA. When you need to calculate from tooling values, use BD = 2 × (R + T) × tan(A/2) − BA, where BA = (π/180) × A × (R + K × T).
At 90°, tan(A/2) = tan(45°) = 1, so the outside setback simplifies to R + T. Calculate BA, then BD = 2 × (R + T) − BA.
Add all finished outside dimensions, then subtract one bend deduction for each bend: Flat Length = Σ outside dimensions − Σ bend deductions.
Bend allowance is the arc length along the neutral axis; bend deduction is the amount you subtract from the outside dimension total to get the flat blank. They reference different points but yield the same flat length when inputs are consistent.
Find the row matching your material, thickness, inside radius, and angle, then read the listed BD value. Subtract one BD per bend from the sum of your outside dimensions to get the flat length. Confirm the chart's K-factor and radius match your tooling before relying on it.
Conclusión
The bend deduction workflow is short and repeatable:
- Confirm material, thickness, radius, angle, and K-factor.
- Calculate bend allowance.
- Calculate outside setback.
- Calculate bend deduction:
BD = 2 × OSSB − BA. - Subtract one bend deduction per bend from the outside dimension total.
- Verify the first piece against the actual press brake setup.
The formula gets you an accurate flat pattern on paper. Consistent tooling, real material data, and a quick test bend get you an accurate part on the floor. As a press brake manufacturer, our advice is simple: calculate carefully, but always let the machine confirm the number before you commit a production run.
Stay Updated on Industrial Innovations
Subscribe to our newsletter for the latest insights on manufacturing technology, sustainability, and industry trends.
