Why several different bends is a different problem
The bend allowance formula is well known and this page uses the same one everyone does. What changes when a part has several bends of different angles is not the formula, it is that bend allowance is not linear in angle, so you cannot work out one bend and multiply. A 90 degree bend and a 45 degree bend in the same material with the same radius have deductions that differ by more than a factor of three, and averaging them produces a blank that is wrong in a way that looks plausible.
The second thing that changes is that the blank length stops being the useful output. You know the total early on. What you need on the brake is where on the blank each bend line sits, because that is what sets the backgauge, and it is where multi-bend parts actually go wrong. This page reports every bend line position from both ends, because a real bending sequence flips the part and the backgauge references whichever end is against it.
The convention used here splits each bend deduction evenly between the two flanges that share it. That places the bend line at the centre of the formed radius, which is the position that matches how a brake operator thinks about it and how CAD flat patterns are normally dimensioned.
Two ways to measure a flange, and only one of them is on your drawing
Flange dimensions come in two flavours and mixing them is the fastest way to produce a wrong blank. Outside mould line dimensions run to the theoretical sharp corner where the two outside faces would meet if the bend had no radius. That is how parts are drawn and how you measure a finished part with a square, and for those you subtract the bend deduction. Tangent dimensions run to the point where the flat stops and the curve begins, and for those you add the bend allowance.
Both routes land on the same blank, which gives you a free check. If the two sets of flange numbers you have do not produce the same blank length through their respective routes, one set was measured the other way. The mode selector on this page switches between them so you never have to convert by hand.
Radius per bend, and why it may not be the drawing radius
Each bend on this page can carry its own inside radius, with a default that fills in for the ones you leave blank. That is not a convenience, it is a necessity, because in air bending the inside radius that actually forms is set mostly by the die opening rather than by the punch nose. Bend the same part in a half inch vee and a one inch vee and you get two different radii and two different deductions from identical tooling settings and identical material.
The practical consequence is that if a part is bent across several different die openings, which happens whenever the flanges vary a lot in length, the bends genuinely have different radii and the flat pattern has to account for it. If they all go in the same vee, one default radius covers everything and the per-bend fields can stay empty.
The single-bend case, along with the derivation of bend allowance, setback and deduction and how to back-solve K from a measured part, is covered in more depth on the bend allowance calculator. This page is the multi-bend layout tool that sits on top of it.
The K-factor question, answered honestly
K-factor is the input people want a table for, and a table is the one thing that cannot honestly be given. It is not a material property. It is a description, after the fact, of where the neutral axis ended up for a particular combination of material batch, thickness, formed radius, die opening, punch geometry and whether the bend was air bent, bottomed or coined. Common working values run from about 0.33 at tight radii in harder material to about 0.50 at generous radii in soft material, with air bent mild steel at a radius near the material thickness landing somewhere around 0.42 to 0.46. Those are starting guesses for the first test piece, nothing more.
The reliable procedure takes ten minutes and one offcut. Cut a strip of the exact material, measure its length precisely, bend it in the exact tooling at the exact angle you will use, then measure the two outside flanges of the result. Subtract the tangent 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-factor, and it is worth more than every published figure combined because it describes your setup rather than somebody else.
Write the result on a card with the material, thickness, tooling and angle it came from, and tape the card to the brake. Over a year that card becomes the most valuable document in the shop.
Bend order, which the arithmetic will not save you from
Four or more bends and the sequence stops being obvious. Each hit has to leave the part in a shape that can still sit on the die for the next one, and the classic failure is a part whose last bend requires a flange that has already been formed to pass through the ram. Working the order out on paper, or with a cardboard mockup, before cutting a nest of blanks costs an hour. Discovering it after cutting fifty costs a lot more.
Related constraints that live in the same place: bends closer together than roughly six times the material thickness interact and the flat pattern drifts, flanges shorter than about the radius plus the thickness have nothing to sit on the die shoulder, holes within about three thicknesses of a bend line pull into ovals, and bends that end at a sheared edge want relief notches or the edge tears. None of those change the blank length, and every one of them can ruin a part with a perfect blank length.
For the tonnage the brake needs to make each of those bends, the press brake tonnage calculator takes the same thickness, radius and die opening. For the material the blanks come out of, the sheet metal gauge chart converts gauge numbers to real thicknesses, and the sheet nesting yield calculator works out how many blanks come off a sheet.
Questions people ask
Why are the bend line positions given from both ends?
Because the backgauge only ever references one end of the blank at a time, and which end that is changes as the part is rotated between hits. A four bend part typically gets flipped at least once, and after the flip the distance you need is measured from the other end. Reading it off a table beats subtracting in your head with a formed part in one hand, and it removes an entire category of error where the right number is applied from the wrong reference. Both columns come from the same layout, so they always agree.
Can I mix different materials or thicknesses in one part?
Not in one calculation, because thickness and K-factor are single inputs that apply to every bend. That is correct for a real part, which is one piece of one material. If you are laying out an assembly of several formed pieces, run each piece separately. What you can mix within one part is angle and radius per bend, which is the case this page exists to handle, and it covers most of what makes a multi-bend part awkward.
What happens if the calculation says the blank is negative or zero?
It means the deductions have consumed more length than the flanges contain, and there are two usual causes. The first is that the flanges really are too short for the thickness and radius, in which case the part cannot be made as drawn without larger flanges or tighter radii. The second, and much more common, is that the flange lengths were measured to the bend tangent while the mode is set to the outside mould line, so a deduction is being subtracted from dimensions that never included it. Switch the mode and see whether the number becomes sensible.
Does the order of the flanges in the fields matter?
Yes, they read as a chain along the blank. Flange 1 is at one end, then bend 1, then flange 2, and so on to the last flange at the other end. The bend line positions are reported from the flange 1 end, and the reversed column from the far end. The angles are the amount each bend turns rather than the included angle between the flanges, which for a right angle means 90 rather than 90 either way, and this page does not track bend direction because up bends and down bends have the same deduction. If your part has bends in both directions, the flat pattern is unaffected and only the bend sequence and tooling clearance care.
How much error does a wrong K-factor actually cause?
Enough to matter and not enough to be obvious, which is the worst combination. On 0.075 inch material with a 0.075 inch radius, a K-factor wrong by 0.10 shifts each 90 degree bend allowance by about 0.012 inches. On a single bend that is invisible. On a six bend enclosure it accumulates to nearly a sixteenth, every bend line has crept, and the part does not close up at the last corner. The error also distributes unevenly across bends of different angles, which is why the part comes out wrong in a way that is hard to trace back to one cause. Test coupon first.