Bend Allowance Calculator — K-factor, bend deduction and flat pattern

When sheet metal is bent, the inside of the bend is compressed and the outside is stretched. Somewhere between the two is a surface whose length does not change, and the whole of flat-pattern arithmetic is about locating it. The bend allowance calculator above finds the arc length along that surface, converts it into the setback and deduction a shop actually works with, and returns the blank length to cut. It will also run the problem backwards and derive the K-factor from a coupon you have already bent and measured.

Arb Digital publishes this as a fabrication and teaching tool. The arithmetic is exact; the input that drives it is not. The K-factor is a property of your material, your tooling and your bending method together, and no chart on any website knows what your press brake does. Everything here is set up so that the uncertainty sits in one clearly labelled input rather than being hidden inside the calculation.

What This Bend Allowance Calculator Does

It computes four related quantities that describe the same bend from different directions. Bend allowance is the arc length of material consumed by the bend, measured along the neutral axis. Outside setback is the distance from the theoretical sharp corner back to the tangent point where the flat leg meets the radius. Bend deduction is how much shorter the flat blank is than the sum of the outside legs. And the flat pattern length is the blank itself.

Which one you use depends on how your drawing is dimensioned. Parts dimensioned to the mould line, the theoretical sharp corner, are laid out with the deduction. Parts dimensioned to the tangent points are laid out with the allowance. Both routes reach the same blank, and the tool prints all of them so that a drawing in either convention can be checked against the other.

The second mode is the one worth having. Enter a coupon's measured flat length along with the legs, radius and angle you achieved, and it solves for the K-factor that reconciles them. That is the only K-factor that means anything for your shop, and it is why this page carries no chart.

How to Use It

1. Measure the achieved inside radius, not the drawn one. In air bending the radius comes from the die opening and the material's springback, so it drifts from the tooling nose radius by a long way.
2. Enter the bend angle in the stated convention — degrees the material turns through, so a right angle is 90. If your drawing gives the included angle between the legs, subtract it from 180 first.
3. Get a K-factor from a coupon. Cut a strip of the same material, thickness and grain direction, measure it, bend it on the machine you will use, and run the K-factor mode.
4. Check the deduction against the allowance. If the two routes disagree, something has been entered in the wrong convention.
5. Prove the flat before you cut a batch. One test part is cheaper than a nest of scrap.

The Formula / How It's Calculated

The neutral axis sits at a radius of r + K t from the centre of the bend, where r is the inside radius, t is the thickness and K is the K-factor. The bend allowance is the arc length of that circle over the bend angle:

BA = (π / 180) × A × (r + K t), with A in degrees. It is nothing more than the arc length of a circle, in the form set out at Wolfram MathWorld's Arc Length entry, applied to the neutral surface.

The outside setback is the tangent geometry at the corner: OSSB = tan(A / 2) × (r + t). The bend deduction is the difference between going round the corner and going through it: BD = 2 × OSSB − BA. And the blank, for outside-dimensioned legs, is flat = A + B − BD per bend.

Running it backwards for K, from a measured flat: the allowance that flat implies is BA = flat − (A + B) + 2 OSSB, and from that K = (BA × 180 / (π A) − r) / t.

Worked example with the loaded values. Thickness 1.5, inside radius 1.5, bend angle 90 degrees, K-factor 0.42. The neutral radius is 1.5 + 0.42 × 1.5 = 2.13, so BA = 1.5708 × 2.13 = 3.3458. The setback is tan 45° × (1.5 + 1.5) = 3.0, so BD = 6.0 − 3.3458 = 2.6542. With outside legs of 50 and 30, the blank is 80 − 2.6542 = 77.3458.

Why There Is No K-Factor Table on This Page

K is not a material constant. It moves with the ratio of inside radius to thickness, and it moves with the forming method. A tight bend in soft material sits at one end of the usual range; a large-radius bend or a coined bend sits at the other. Two shops bending the same coil to the same drawing with different die openings will need different K-factors, and both will be right for their own machine.

There is a second trap, which is that the symbol is not defined identically everywhere. The convention used here, and in mainstream CAD systems, is that K is the distance from the inside surface to the neutral axis expressed as a fraction of the full thickness, so it runs from 0 to 0.5. The German standard DIN 6935, Cold bending of flat rolled steel products, defines its correction factor against half the thickness instead, so a value taken from a DIN table cannot be typed straight into a CAD field expecting the other definition. If you are handed a bare number with no definition attached, the first job is to find out which one it is.

That is why this tool takes K as an input and gives you a way to measure your own. The whole point of a test coupon is to fold all of the unknowns — alloy, temper, rolling direction, die opening, punch radius, springback, machine wear — into one number that is true for the setup you actually have. Recording that number against the material and tooling combination, and re-checking it when either changes, is what separates a shop that hits size first time from one that trims every part.

Air Bending, Bottoming and Coining

The forming method changes the bend more than the material does. In air bending the punch never presses the sheet fully into the die; the part is formed by three-point contact and the inside radius is governed by the die opening, following the rule of thumb that the natural radius is a fraction of that opening. Springback is significant and varies with the sheet, so the angle has to be overbent. K tends toward the lower part of its range.

In bottoming the sheet is pressed onto the die walls, so the angle is set by the tooling and springback is much reduced. In coining the punch is driven into the material hard enough to plastically set the inside radius, springback is nearly eliminated, and the neutral axis moves outward toward the middle of the thickness, pushing K toward 0.5. The tonnage required rises steeply from air bending to coining, which is why most production work is air bent despite the extra variability.

Grain direction matters too. Bending across the rolling direction is more forgiving than bending along it, and on some alloys and tempers bending parallel to the grain will crack at a radius that is perfectly safe across it. Minimum bend radius is a material property published by the mill, not something a geometry page can supply.

Where the Flat Pattern Goes Wrong in Practice

Four things account for most scrapped blanks. The first is the angle convention: a part drawn with a 120 degree included angle is a 60 degree bend, and entering 120 produces a blank that is wildly wrong. The second is dimensioning: mixing outside dimensions on one leg with tangent-point dimensions on the other quietly adds or drops a setback. The third is bends that are too close together, where the flat portion between them is shorter than the setback and the two bend zones overlap — no flat-pattern arithmetic is valid there, and the part needs a different sequence or a different tool. The fourth is holes near a bend, which distort as the material moves; they either need to sit outside the deformation zone or be punched after forming. Our clearance hole calculator covers the hole sizing itself, and the bolt circle calculator sets out patterns of them.

It is also worth being clear about units. The arithmetic is unit-agnostic — it works in millimetres or in inches as long as everything is consistent — but a flat pattern that mixes the two is a familiar way to scrap a sheet. The conventions for writing and converting units are set out in NIST Special Publication 811, the Guide for the Use of the International System of Units. For estimating the material a nest consumes, our material weight calculator converts area and thickness into mass, and the cross-sectional area calculator handles the section geometry of the formed part.

Common Mistakes to Avoid

• Entering the included angle instead of the bend angle — they add to 180, and swapping them changes the blank by more than any tolerance will absorb.
• Using the drawn radius instead of the achieved one — in air bending the inside radius comes from the die opening, so it is measured on the part, not read off the tooling.
• Taking a K-factor from a chart without checking its definition — the CAD convention measures from the inside surface against full thickness; DIN 6935 uses a different reference.
• Mixing dimensioning conventions across a part — outside legs on one side and tangent points on the other silently adds or drops a setback.
• Placing bends or holes too close together — overlapping bend zones and distorted holes are geometry problems no flat-pattern formula can fix.

Related Free Tools From Arb Digital

Size the fixings with the clearance hole calculator, lay their positions out with the bolt circle calculator, work out the tightening with the bolt torque calculator, and estimate material with the material weight calculator. For angled cuts in flat or round stock, use the angle cut calculator, and for the trigonometry behind the setback, the trigonometric functions calculator. Everything we publish is on the free online tools hub.

Frequently Asked Questions

This tool applies published flat-pattern geometry to values you supply, for fabrication planning and education. The K-factor is a property of your material and your machine, so results should be proved on a test coupon before any batch is cut.