How this instrument works
Bend allowance is the length of flat stock a bend itself consumes — not the two straight legs on either side, but the curved region between them. Bend a sheet and every fibre through its thickness travels a different distance around the curve: the outside surface stretches, the inside surface compresses, and exactly one surface in between, the neutral axis, keeps its original length. Bend allowance is the arc length that surface sweeps through, BA = θ · (R + K·T): an angle in radians times the radius out to that neutral surface, because arc length is always angle times radius.
The K-factor is what makes this formula shop-specific rather than universal. It reports where the neutral axis actually sits, as a fraction of thickness measured in from the inside face, and that position moves. On a tight bend the inside material is compressed hard enough to thicken measurably, dragging the neutral axis toward the inside surface and pushing K down toward 0.3; on a gentle, wide-radius bend the sheet barely notices the difference between inside and outside, and K drifts up toward 0.5. A common shop rule sets K = 0.33 whenever the inside radius is under about twice the stock thickness, and K = 0.5 once it exceeds that — a coarse two-step stand-in for a curve that is actually continuous.
The formula assumes a clean circular arc under simple bending, with one K-factor holding across the whole curve — true enough for air-bent sheet metal at ordinary radii, less true once the inside radius drops below roughly one material thickness. Below that point the inside fibre is compressed hard enough to risk folding rather than curving, published K-factor tables start disagreeing with each other by a wide margin, and many shops simply forbid a radius that tight, turning to hemming, coining, or a redesigned flange instead. Bend allowance also says nothing about springback, the small unbending a part does the instant the press releases it, which gets applied as a separate correction after the flat pattern is cut.
- Enter the included Bend angle — how far the sheet actually turns through the bend, in degrees by default; switch the unit menu to radians if that's what your flattening software exports.
- Enter Inside bend radius, measured to the concave face of the bend — the punch-nose radius that presses into the sheet, not any outside radius.
- Enter Material thickness for the sheet stock itself, before bending.
- Set K-factor: roughly 0.33 for a tight bend where the inside radius is under about twice the thickness, closer to 0.5 for a gentler one, or a value pulled from your own bend-deduction chart.
- Read Bend allowance and add it to your flat-pattern leg lengths, measured to their bend tangent lines, to get the total flat blank length.
Worked example — a 90-degree bend in 2 mm sheet
Take 2 mm mild steel bent 90 degrees around a punch that leaves a 3 mm inside radius — an ordinary line on a press-brake job sheet. Enter 90 into Bend angle, 3 into Inside bend radius, 2 into Material thickness, and 0.33 into K-factor. That 0.33 is the usual shop figure for bends where the inside radius sits under about twice the stock thickness, which this one does: 3 mm against a 4 mm threshold.
Internally 90 degrees becomes 1.5707963267949 radians, and Bend allowance works out to θ · (R + K·T) = 1.5707963267949 × (0.003 + 0.33 × 0.002) = 1.5707963267949 × 0.00366 = 0.00574911455607 metres, which is 5.749115 mm. That is the length of neutral-axis material the bend consumes — not the outside surface, which stretches further getting around the corner, and not the inside surface, which is squeezed shorter.
A flat pattern built from two 20 mm legs, each measured to its bend tangent line, is not 40 mm of stock. It needs those two legs plus the 5.749115 mm bend allowance for the one bend between them: 45.749115 mm in total. Leave the allowance out of the layout and the finished bracket comes back roughly 5.7 mm short across that corner — a shortfall workshops learn to recognise on sight.
Questions
What exactly is bend allowance measuring?
The arc length of the neutral axis — the one surface inside the sheet thickness that neither stretches nor compresses — as it sweeps through the bend. It is the flat stock the bend itself consumes, above and beyond the two straight legs on either side, and it is what gets added into a flat-pattern layout so the finished, bent part comes out the length it was designed to be.
Why isn't K-factor just 0.5, the exact middle of the thickness?
Because bending is not symmetric. The inside face is squeezed and thickens slightly while the outside face stretches and thins, so the surface that keeps its original length sits closer to the inside than the geometric mid-plane, especially on tight radii where that compression zone dominates. K = 0.5 describes only a very gentle, wide-radius bend; most sheet-metal work sits nearer 0.3 to 0.4.
Where does the 0.33-versus-0.5 rule of thumb come from?
It is a shop-floor shortcut, not a law of physics. Many bend-deduction charts set K near 0.33 once the inside radius drops under about twice the material thickness, and nearer 0.5 once it exceeds that, because a tight radius pushes more material into plastic compression on the inside face. Real K-factors trace a continuous curve against radius-to-thickness ratio, material, and bending method; the rule is a coarse two-step stand-in for that curve.
Does bend allowance depend on which way I measure the angle?
Yes, by convention. This formula wants the included bend angle — how far the sheet actually turns, measured as the change in direction through the bend — not its complement. A sharp 90-degree corner turns the sheet through 90 degrees, so enter 90; a shallow 30-degree kink turns it through only 30. Confusing bend angle with flange angle, since the two sum to 180 degrees, is the most common input mistake.
How is bend allowance different from bend deduction?
One is added, the other subtracted. Measure flat-pattern legs to the sharp corner point they would meet at if the bend had zero radius, and you subtract a bend deduction from their sum. Measure legs instead to the bend's tangent lines — where flat stock ends and the curved region begins — and you add this bend allowance on top. Mixing the two conventions in one layout is the fastest route to a part the wrong length.
What breaks down at very tight bend radii?
The neutral-axis picture itself starts to fail once the inside radius drops below roughly one material thickness. Compression on the inside face grows severe enough to risk cracking on the outer fibre, published K-factor charts stop agreeing with each other by a wide margin, and many fabricators simply avoid specifying a radius that tight, switching instead to hemming, coining, or a redesigned flange.