Sheet Metal Bend Allowance Calculator

What bend allowance is and why the blank is never the sum of the legs

Fold a strip of steel and you have not simply rotated two flat legs about a corner. Inside the bend the metal is squeezed and gets shorter; outside it is stretched and gets longer. Somewhere between the two faces there is a surface whose length does not change at all. That surface is the neutral axis, and its arc length through the bend is the bend allowance.

This matters because a flat pattern is built from lengths, not from angles. If you cut a blank equal to the sum of the finished leg dimensions, the part comes off the press brake too long, every time, by an amount that grows with thickness and with the number of bends. A five-bend enclosure laid out without allowances can miss by a quarter of an inch, which is enough to make the lid stop fitting.

The neutral axis does not sit at mid-thickness. Compression on the inside is resisted more stiffly than tension on the outside, so the unstretched surface migrates toward the inside face, and the tighter the radius the further it moves. The K-factor is the single number that captures where it ended up: it is the distance from the inside face to the neutral axis, expressed as a fraction of material thickness. K = 0.5 puts the neutral axis exactly at mid-thickness; K = 0.33 puts it a third of the way in. Once you know K, the geometry is elementary.

The formula, term by term

Arc length equals radius times angle in radians. That is the whole derivation. The radius of the neutral axis is the inside radius plus the K-factor offset, R + K·T, and the angle turned through, converted to radians, is A × π / 180. Multiply them:

BA = (π / 180) × A × (R + K·T)

Read the terms in the order they bite. T is the real measured thickness — nominal 16 gauge steel is 0.0598 in but coil varies, and a thousandth of error here is multiplied by K and by the angle. R is the inside radius you actually achieve, which on an air bend is set by the die opening rather than by the punch. A is the angle the metal turns through, so a square corner is 90°, not the 90° included angle a machinist might read off a print — the two happen to coincide at a right angle but diverge everywhere else, and this is the single most common data-entry error on this page. K is the only term that is empirical.

Two companion quantities fall out of the same geometry. Outside setback is the distance from the bend tangent line to the apex where the two outside faces would meet if extended: OSSB = tan(A/2) × (R + T). Bend deduction is what you subtract from the sum of outside mould-line dimensions: BD = 2 × OSSB − BA. Use bend allowance when your dimensions run tangent-to-tangent, and bend deduction when your print is dimensioned to the outside corners, which is how most fabrication drawings arrive.

At 180° the tangent of half the angle is undefined, so setback and deduction have no finite value on a hem. The bend allowance is still perfectly well defined — it is simply π × (R + K·T) — so lay a hem out from the allowance.

Choosing a K-factor you can defend

The K-factor is where measurement beats theory. Every other term in the formula you can read off a print or a micrometer; K you have to earn. The practical range for ordinary air bending in steel and aluminium is roughly 0.38 to 0.46, and 0.42 is a defensible starting point for cold-rolled steel at radii near one material thickness.

Three effects push it around. Tighter radii move the neutral axis inward, so K falls as the R/T ratio falls — below R/T = 1 you are into the range where published tables disagree with each other and with your machine. Harder or more work-hardened material also lowers K. And the forming method matters: coining, which drives the punch into the material, produces a different K than air bending the same part, because the metal is being locally thinned rather than simply wrapped.

The only reliable procedure is to back-solve K from a test bend. Cut a strip of known length, bend it once, measure the outside dimensions, compute the bend deduction you actually got, and rearrange the two formulas to find the K that produces it. Ten minutes of this at the start of a production run is worth more than any chart, and it is what shops that hit tolerance on first-article inspection actually do. Once you have a K for a given material, thickness, tooling and angle, record it — the number is a property of that combination, not of the alloy alone.

Interpreting the output is simple: bend allowance is always positive and always less than the outside path but more than the inside path around the corner. If your calculated allowance comes out larger than the sum of the two setbacks, the bend deduction goes negative. That is not an error — it happens on open bends of less than about 60° with generous radii, and it means the blank must be longer than the sum of the outside dimensions.

Bend allowance and deduction for 90° bends, R = T, K = 0.42

Valid only for the stated conditions: 90°, inside radius equal to thickness, K = 0.42. Change any of the three and recompute rather than scaling these numbers.

Mistakes that put a flat pattern out of tolerance

• Entering the included angle instead of the angle turned through. A 30° included angle is a 150° bend. The two are equal only at 90°, which is exactly why the error survives the first job and appears on the second.
• Using the punch radius as the inside radius. In air bending the inside radius is governed by the die opening, roughly 16% of it in mild steel, and a sharp punch in a wide die produces a much larger radius than the punch nose suggests. Measure the radius on a sample bend.
• Trusting a gauge number for thickness. Sheet is sold to a tolerance. A 0.003 in difference on 16 gauge shifts the allowance by about 0.002 in per bend, which accumulates across a six-bend part.
• Carrying one K-factor across materials. A K measured on cold-rolled steel does not transfer to 5052 aluminium or to 304 stainless on the same tooling.
• Mixing bend allowance and bend deduction in the same layout. Allowance is added to tangent-to-tangent flats; deduction is subtracted from outside mould-line dimensions. Use one convention for the whole part.
• Ignoring springback. Bend allowance predicts length, not angle. The part will spring open by one to several degrees depending on alloy and radius, and you overbend to compensate. That overbend does not change the developed length appreciably, but it does change the radius you end up measuring.

Where this fits among the other press brake numbers

Bend allowance is one of three calculations that have to agree before a part runs. The second is force: the brake has to be able to close the bend at all, which you check with the press brake tonnage calculator. That page also gives you the die opening and the resulting inside radius, which feed straight back into this one — you cannot pick an inside radius independently of the tooling you have. The third is the full layout, which for anything with more than one bend is easier in the sheet metal flat pattern calculator, where the allowances are summed for you.

Older shop practice used bend-allowance charts published per gauge and per angle rather than a K-factor. Those charts encode a particular K implicitly, usually near 0.44 for the aircraft-industry tables and near 0.33 for tighter tooling assumptions. They are still perfectly usable, but they are opaque: when a part comes out wrong you cannot see which assumption failed. The K-factor form exposes the one empirical number so you can measure and correct it.

CAD systems all implement this same equation, though they name things differently. SolidWorks and Inventor let you supply K-factor, bend allowance or bend deduction per bend, and a bend table is simply a lookup of the same quantities by thickness and angle. If your CAD flat pattern and your hand calculation disagree, the discrepancy is almost always a different K or a different inside radius, not a different formula.

Once the blank length is settled, the remaining shop questions are material-related: what the blank weighs for shipping and cost, which the steel plate weight calculator answers, and whether the bend will crack, which comes down to minimum bend radius for the alloy and temper and to bend-line orientation relative to the rolling direction.

Key terms

Neutral axis

The surface through the thickness that is neither stretched nor compressed by the bend. Its arc length is the bend allowance.

K-factor

Distance from the inside face to the neutral axis divided by material thickness. Always between 0 and 0.5 for a real bend.

Tangent line

The line where the flat portion of a flange stops and the bend radius begins. Flat segment lengths are measured tangent to tangent.

Outside mould line

The imaginary apex where the two outside faces would meet if the radius were removed. Prints are commonly dimensioned to it.

Y-factor

An alternative to K used in some aerospace tables, equal to K × π/2. It folds the radian conversion into the constant.