Bend Allowance and Bend Deduction

Bend allowance and bend deduction are the two numbers that decide whether a flat pattern produces a part that measures correctly after forming. This guide covers both formulas, the K-factor behind them, worked numbers you can check line by line, and a chart of ready values for 90° bends in 1.0 to 3.0 mm sheet.

Why the Flat Pattern Is Not the Sum of the Flanges

When sheet bends, the material on the outside of the bend stretches and the material on the inside compresses. Neither surface keeps its original length. Somewhere between them there is a surface that does keep its length, and that surface is where the flat pattern has to be measured from.

That single idea produces both numbers used in the shop. If you build the flat pattern by tracking that surface through the bend, you are using bend allowance. If you start from the outside dimensions on the drawing and subtract the material that the bend consumes, you are using bend deduction. They describe the same bend from opposite ends.

What Bend Allowance, Bend Deduction and K-Factor Mean

Bend allowance (BA)

The length of the neutral surface consumed by the bend, measured along its arc. It is the arc length, not a straight distance, which is why it depends on the bend angle and not only on the radius.

Bend deduction (BD)

The amount subtracted from the sum of the outside dimensions to get the flat length. It is the difference between measuring around the outside corner and measuring along the neutral surface.

K-factor

Where the neutral surface actually sits inside the thickness, expressed as a fraction of the thickness measured from the inside face. It ranges from 0 to 0.5, and it is the only input in the calculation that cannot be derived from the drawing. Typical published values are around 0.33 for mild steel, 0.44 for stainless in air bending, 0.33 for soft aluminium and 0.40 for harder aluminium grades, with bottom bending sitting higher than air bending. Those are starting points, not constants, and the section on determining K-factor below explains why.

Bend Allowance Formula

The bend allowance formula takes the angle in degrees, the inside radius and the thickness, and returns the arc length of the neutral surface through the bend:

BA = θ × (π / 180) × (R + K × T)

The π / 180 converts degrees into radians. That conversion is the first place a spreadsheet goes wrong: if the software expects radians and gets degrees, the answer is out by a factor of 57.

Bend Deduction Formula

Bend deduction starts from the outside dimensions, which is how most drawings are dimensioned. It needs the outside setback first:

OSSB = tan(θ / 2) × (R + T)
BD = 2 × OSSB − BA

Inside setback is the same quantity measured from the inside face, and it equals tan(θ / 2) × R. The two setbacks differ by exactly tan(θ / 2) × T, which is the material thickness projected across the corner.

Bend Allowance vs Bend Deduction: Which One to Use

They are not alternatives, and they are not competing methods. Pick the one that matches how the part is dimensioned, and check the result against the other.

One relationship is worth remembering because it catches arithmetic mistakes: for the same bend, 2 × OSSB − BD = BA. If a flat pattern reaches the shop and that identity does not hold, one of the three numbers was copied from a different bend.

Bend Allowance and Bend Deduction Chart for 90° Bends

The table below is the arithmetic from the formulas above, computed for a bend angle of 90° and a K-factor of 0.40. It is here so you can sanity-check a program output quickly, not as a substitute for a test bend.

Two patterns are visible in the numbers, and both match what happens on the machine. First, at a fixed radius, increasing the thickness increases both BA and BD, because the neutral axis moves outwards and the outside corner gets larger. Second, at a fixed thickness, increasing the radius increases BA faster than it increases BD, because more of the bend is arc and less is corner.

Note on the K-factor used here: the chart is calculated with K = 0.40 throughout, which is a reasonable starting value when the inside radius is between one and two times the thickness. If your tooling gives a different K, substitute it into the formula. The R / T column tells you when you are outside that band, and step back to the K-factor section below.

Bend Allowance Calculator

Enter the bend and the two flange dimensions, and the calculator returns the flat length using the formulas on this page. Flange dimensions are taken on the outside faces, which is how most drawings are dimensioned; if your drawing dimensions inside, set the inputs accordingly or subtract R + T from each outside value first.

The default values are the worked example below, so you can compare the output with the table further down the page before you trust it with your own numbers.

K-Factor: Where the Uncertainty Sits

The K-factor is the part of this that cannot be looked up reliably. Typical values sit near 0.33 for a radius below the material thickness, around 0.38 to 0.42 when the radius is one to two times thickness, and approach 0.5 for larger radii. We refine it empirically per material batch using test bends, because two parts cut from different coils can differ enough to move the flat pattern by a tenth of a millimetre, which matters when a hole sits near a bend.

Determining the K-factor experimentally

Cut a blank of known length, bend it to a known angle in the production tool, then measure the resulting flanges. From the measured flanges, work back to the actual bend allowance, and from there back to the K-factor. The result is specific to that material, that thickness and that die, which is exactly why it is more trustworthy than a published table. We do this for new material batches and for any part where a hole or slot sits close to a bend.

Is a K-factor of 0.33 always right for mild steel

No. It is a common starting value for tight radii, and it becomes optimistic as the radius grows. The ratio that matters is R divided by T, not the material name alone. A 1.0 mm radius in 3.0 mm mild steel and a 3.0 mm radius in 3.0 mm mild steel behave differently even though the material is the same.

Flat Pattern Length for Parts With Several Bends

For a part with more than one bend, the flat pattern is the sum of every straight section plus the bend allowance of every bend. Add them in order along the part, and do not apply a single bend deduction multiplied by the number of bends, because each bend has its own radius and angle.

Two shortcuts cause most of the errors we see on multi-bend parts. The first is summing outside dimensions and subtracting one deduction per bend, when two of the bends share a flange: the shared flange is counted twice. The second is using a variable radius, where the inside radius changes between bends because the tooling changed mid-part. Variable radii need a separate calculation for each bend, and on tight-tolerance parts we confirm each one rather than averaging them.

Common Errors That Move the Flat Pattern

• Degrees entered where radians are expected. The error is large and consistent, which is how it gets caught: every part in the batch is wrong by the same proportion.
• Using the nominal thickness instead of the actual. Sheet tolerance is real. On a 2.0 mm specification the actual can sit at either end of the range, and the neutral axis moves with it.
• Assuming the die gives the radius on the drawing. Air bending sets the inside radius from the die opening, roughly 0.16 times V for common tooling, which often differs from what the drawing states.
• Copying a K-factor between materials. Stainless and aluminium do not share the mild steel value, and neither do different tempers of the same aluminium grade.
• Mixing inside and outside dimensions in one formula. A drawing dimensioned outside with one flange treated as inside will be out by 2 × (R + T) on that flange, which is a visible error, not a rounding error.
• Applying one deduction to a bend of a different angle. Deduction for a 90° bend does not scale linearly to 120°.

A Worked Example, End to End

Formulas are easier to trust once you have seen them run on a real part. The example below is a 2.0 mm SPCC bracket with a single 90° bend, formed in a 16 mm die. Both flanges are dimensioned on the outside faces, which is how most drawings arrive.

What Buyers Usually Ask About Bend Allowance Bend Deduction

Should the drawing dimension flanges inside or outside?

Whichever way your inspection will check them, as long as it is stated. We convert either way; what causes problems is a drawing dimensioned outside while someone inspects inside.

Do you use bend allowance or bend deduction?

Both, because they answer different questions. Deduction is used when you start from outside dimensions, allowance when you are building the flat from the neutral axis. Either leads to the same flat length if the inputs agree.

Why do two suppliers quote different flat lengths for the same part?

Different assumed K-factors and different die openings. Neither is wrong until the die is fixed, which is why we confirm the tool set before releasing a program.

What is the difference between bend allowance and bend deduction in one sentence?

Bend allowance is the arc length of the neutral surface through the bend, and bend deduction is how much shorter the flat is than the sum of the outside dimensions. The first is added, the second is subtracted, and both give the same flat length for the same bend.

Do I need to calculate this if the CAD software already flattens the part?

The software will produce a flat pattern with whatever K-factor is loaded in its bend table, and that value is often a default rather than your tooling. Calculating one bend by hand is the quickest way to find out whether the value in the software matches the press. On parts where a hole lands within a millimetre of a bend, it is worth the two minutes.

Questions about a specific part are usually faster to answer against the drawing — send it through the review route below.

Before you send the RFQ. Reference radius assumptions behind the allowance first if this part is still at drawing stage, because most cost drivers on a bent part are set there. For anything already specified, flat pattern development is where to send it. Related: bending theory and K-factor, drawing review before quoting, bending tolerance standards, multi-bend sequences and bend design for manufacture.