The three numbers and what each one is for
Sheet metal bending generates three related figures and people mix them up constantly, so it is worth being precise about which is which.
Bend allowance is the length of material consumed inside the bend itself, measured along the neutral axis. It is what you add to flange lengths that were measured up to where the flat stops and the curve starts, the bend tangent. The formula is the arc length of a circle: the bend angle in radians times the radius of the neutral axis, which sits at the inside radius plus K times the thickness.
BA = angle in radians x (inside radius + K x thickness)
Outside setback is the distance from the bend tangent out to the outside mould line, the imaginary point where the two outside faces would meet if the bend were sharp. It is tan(angle/2) times the radius plus the thickness. For a 90 degree bend the tangent of 45 is 1, so setback is simply radius plus thickness, which is why 90 degree work feels easy and everything else does not.
Bend deduction is twice the setback minus the bend allowance. It is what you subtract when your flange dimensions were measured the normal way, outside mould line to outside mould line, which is how parts are drawn and how you measure a finished part with a square. Both routes land on the same blank, which is a good check on your arithmetic: if outside dimensions minus BD does not equal tangent dimensions plus BA, one of the two sets of flange figures is wrong.
A worked case, because the arithmetic is easier to trust when you have seen it come out: 0.125 inch material, 0.125 inch inside radius, 90 degrees, K of 0.44. The neutral radius is 0.125 + 0.44 x 0.125, which is 0.180. Bend allowance is 1.5708 x 0.180, which is 0.2827. Setback is 0.125 + 0.125, which is 0.250. Deduction is 0.500 minus 0.2827, which is 0.2173. Two 2 inch outside flanges therefore come off a blank of 4 minus 0.2173, which is 3.7827 inches.
The K-factor is measured, not looked up
This is the part that trips up everyone coming to press brake work from CAD. The K-factor is not a material constant you can find in a handbook and trust. It is a description, after the fact, of where the neutral axis happened to sit for one particular combination of material, thickness, inside radius, die opening, punch geometry and forming method. Change the die from a 0.5 inch vee to a 1 inch vee and the inside radius changes, and so does K. Bottom the part instead of air bending it and K changes again. Buy the same nominal material from a different mill and it can move.
| Situation | K commonly lands near |
|---|---|
| Tight radius, r/t well under 1, harder material | 0.30-0.38 |
| Air bending mild steel, r roughly equal to t | 0.40-0.46 |
| Generous radius, r/t above about 3, soft material | 0.45-0.50 |
| Bottoming or coining | Shifts toward 0.5, and the radius itself changes |
Treat the table as a starting guess only. The reliable procedure takes ten minutes: cut a strip of the exact material you are going to use, measure it, bend it in the exact tooling at the exact angle, measure the two outside flanges of the result, and back-solve. Subtract the tangent-line flange lengths from the measured flat, divide by the bend angle in radians, subtract the inside radius, divide by the thickness. That is your K, for that setup, and it will beat anything you read on the internet including this page.
Why bend radius is not what the drawing says
In air bending, the inside radius that forms is determined mostly by the die opening, not by the punch nose. The usual approximation is that the inside radius comes out around 16 percent of the vee width for mild steel, more for stainless, less for aluminium. So a 0.5 inch vee gives roughly a 0.080 inch inside radius regardless of whether the punch tip is 0.030 or 0.060, as long as the punch is sharper than the forming radius. If the drawing calls a radius and the tooling forms a different one, the drawing loses, and your bend allowance has to be calculated on the radius you actually get.
This is the single most common reason a flat pattern is right on paper and wrong on the floor. Measure the radius on a test bend with radius gauges or by measuring the flat length and back-solving, and use that.
Multiple bends, and where it stops being simple
The bends field multiplies the deduction by the number of identical bends, which is correct as long as they really are identical: same angle, same radius, same direction of measurement, and far enough apart that the forming zones do not interact. Bends closer together than roughly six times the material thickness start to distort each other and the flat pattern drifts. Bends of different angles or radii need to be calculated separately and the deductions summed, because BA and BD are not linear in angle.
Also outside this calculation: springback, bend reliefs at the ends of a flange, grain direction, and the fact that a bend near a hole will move the hole. Springback in particular means the angle you set on the brake is not the angle you get, and the correction is another empirical number specific to your material and tooling. None of that changes the blank length, which is what this page computes, but all of it changes whether the finished part is in tolerance.
Before you cut the sheet
Run the numbers here, then bend a test piece from the offcut of the same sheet, in the same tooling, in the same direction, and measure it. If the test lands where the calculation said, cut the real blanks. If it does not, back-solve the K-factor from what you measured, put that number in the field, and run it again. Ten minutes of scrap is cheaper than a nest of parts that are all uniformly three-sixteenths short, and unlike the parts, the scrap does not have your name on the tag.
Questions people ask
What is a good default K-factor if I have no way to test?
For air-bent mild steel with an inside radius close to the material thickness, 0.44 is a defensible starting point and is what this page defaults to. For thicker plate with a proportionally larger radius, drift up toward 0.46 or 0.50. For hard tempers and tight radii, drop toward 0.35. Understand what you are accepting: a K-factor guess wrong by 0.10 on 0.125 inch material shifts the bend allowance by about 0.020 inches per bend, which is fine for a bracket and not fine for anything that has to line up with existing holes. If the part matters, test.
Bend allowance or bend deduction — which one do I use?
It depends only on how you measured the flanges. If you took the dimensions from a drawing, or measured a finished part with a square, those are outside mould line dimensions and you subtract the bend deduction. If you measured from the end of the flat to where the material starts to curve, those are tangent dimensions and you add the bend allowance. Both give the same blank. The mode selector on this page switches between them so you do not have to convert by hand, and the fact that both routes agree is a useful check that your inputs are consistent.
Why is my finished part the right length but the wrong angle?
Springback. The flat pattern controls length; it has nothing to say about angle. Metal bent past yield partially returns when the punch lifts, so a brake set to 90 gives you 91 or 92 in mild steel and rather more in stainless or hard aluminium. The usual fixes are to overbend by a measured amount, to bottom or coin the bend rather than air bend it, or to use a brake with angle measurement and correction. Whichever route you take, the compensation figure is specific to your material and tooling and has to be established on scrap.
Can I use the same K-factor for aluminium and stainless as for steel?
No, and it will not be a small error. Stainless work-hardens rapidly and springs back much harder, and the inside radius that forms in a given die is larger than for mild steel, which changes both terms in the bend allowance. Aluminium in a T6 temper wants a generous radius and can crack at ratios that mild steel shrugs off, and its K tends to run lower at tight radii. Establish the number separately for every material and thickness you work in regularly, write them on a card, and tape the card to the brake.
How close to an edge or a hole can I bend?
As a working rule, keep holes at least two and a half to three times the material thickness plus the bend radius away from the bend line, or the hole will pull into an oval. Flanges shorter than about the inside radius plus the thickness have nothing to sit on the die shoulder and will either not form or will form somewhere other than where you marked. Bends that end at a sheared edge want a relief notch cut at each end, roughly the material thickness wide and slightly deeper than the radius, or the edge tears. None of these are governed by the flat pattern arithmetic, but every one of them will ruin a part that had a perfect blank length.