Guides — Bend Allowance

Bend allowance and K-factor, explained plain

By Jon Chacon · October 22, 2026

If your flanges keep coming up a little long or a little short while the bend itself looks fine, your flat pattern is wrong — and it’s almost never the brake’s fault. The flat is wrong in the bend, in the small piece of material that ends up curved.

That piece of material has a name and a number. The name is bend allowance. The number hangs on a factor called K. This page is what both of them are, how the math runs, and how to get a number you can trust on your own material.

What bend allowance is

When sheet bends, the outside of the bend stretches and the inside compresses. Somewhere in between there’s a layer that does neither — the neutral axis. Bend allowance is the length of that layer through the bend: the amount of flat stock that actually ends up in the curve.

Your flat blank is the two straight legs — each one measured up to where the bend starts — plus the bend allowance. Get the allowance wrong and the blank is wrong by that amount, taken out of the legs. That’s why a bad number shows up as both flanges being a little off, instead of one big obvious miss.

The formula

Bend allowance = (π ÷ 180) × bend angle × (inside radius + K-factor × thickness)

Three of those you know off the print: the angle, the radius, the thickness. K is the one you have to bring yourself. It’s covered next — first, the math with a real set of numbers.

The worked example

Take the bend from our tonnage example: a 90-degree bend in quarter-inch material (0.250″ thick), 0.375″ inside radius, and a K-factor of 0.44. The arithmetic, step by step:

So that bend uses 0.762 inches of flat. Cut the blank with 0.70 allowed for the bend instead and the part is short before it ever gets to the brake — and the shortage comes straight out of your flanges.

K-factor in plain terms

K is just where the neutral axis sits, written as a fraction of the thickness measured from the inside face of the bend. K = 0 would put the axis right on the inside surface. K = 1 would put it on the outside surface. It’s never either one — the axis sits in between, pulled in from the middle toward the inside face.

For air-bent mild steel, K usually lands around 0.42 to 0.46. That’s the range most shops work in, and it’s why 0.44 is in the example — it’s a fair starting number, not a magic one.

What moves K

One more thing feeds the radius in that list: in air bending, the radius is made by the die opening, not the punch. That’s a setup decision, and it’s written up in Picking a V-die for air bending.

Bend deduction: the same bend, measured from outside

If your dimensions run to the outside of the flanges — to the mold line, where the two outside faces would meet if they kept going — you don’t add the allowance, you subtract the deduction. Bend deduction = 2 × outside setback − bend allowance, and the outside setback is tan(angle ÷ 2) × (inside radius + thickness).

Same bend as the example: tan(45°) × (0.375 + 0.250) = 1 × 0.625, so the setback is 0.625″. Twice that is 1.250. Minus the 0.762 allowance gives a bend deduction of 0.488″. Flat blank = outside flange + outside flange − 0.488, for each bend. Same bend, same blank — just figured from the other side of the lines.

The honest part

Every K chart ever printed is a starting point, including the ranges on this page. K moves with the radius your die actually produces, the lot of material in front of you, and the machine. The way you nail it down is a test bend: cut a strip of the actual material at a known width, bend it, measure what you get, and work the formula backwards to your K. Ten minutes with a test strip, once per material, beats arguing with a chart for the life of the job.

Questions we get asked

Can I use one K-factor for everything?

No. K moves with the radius, the thickness, the material, and how you’re bending. One number for everything guarantees some jobs come out wrong — usually the ones with tight radii, where K drops the most. Keep a number for each material and radius range you run, taken from your own test bends, and you’ll be close every time.

Why did my flat pattern come up short on both flanges?

Because the bend took more material than you allowed for it. When the allowance is under-figured, the bend pulls the difference out of the legs, so both flanges lose a little instead of one losing a lot. Check the radius you’re actually getting first — in air bending the die picks the radius, not the print — then re-check your K against a test bend in the same material.

Does K-factor change in stainless?

Yes. Material moves it, radius moves it, and stainless behaves differently from mild steel under the punch — it work-hardens as it bends and springs back more. Don’t carry your mild-steel K into a stainless job and expect the flat to come out. Test-bend the stainless and figure its own number.

Where does the inside radius in the formula come from?

In air bending, from the die. The radius forms off the V-opening — roughly 16% of the opening in mild steel — not off the punch, as long as the punch is smaller than that natural radius. So the radius in the bend-allowance formula is the one your die produces, which is why die selection and flat patterns are the same conversation.

Run your own numbers — free 14-day trial, no credit card.

Start Your Free Trial