What a flat pattern is and why it is shorter than the part
The flat pattern is the two-dimensional blank a bent part came from. Cut it, form it on the brake, and the finished dimensions land where the drawing says. Get it wrong and every downstream feature moves — holes shift relative to bend lines, flanges finish long or short, and an enclosure stops closing.
The reason the blank is not simply the sum of the finished legs is that each bend consumes material. Inside the bend the metal compresses and outside it stretches, and only one surface through the thickness keeps its original length. The arc of that surface is the bend allowance, and it is always shorter than the path around the outside of the corner. Dimension a part to its outside mould lines and you are measuring to imaginary sharp corners that the real bend never reaches, so you must subtract a bend deduction for each bend.
Every bend crossed by the unfold contributes one deduction. A simple L has one, a U-channel has two, a hat section has four, and a box formed from a single blank has bends in both directions — unfold each direction separately, because a bend that runs parallel to the direction you are measuring does not consume any length in that direction.
Two routes to the same blank, and why they agree
Which formula you use depends on how your print is dimensioned, not on the part.
From outside mould lines. Most fabrication drawings dimension to the outside corners, which is what a caliper on the finished part measures. Add up those dimensions and subtract one bend deduction per bend: L = Σdoutside − n × BD.
From tangent-to-tangent flats. A CAD flat pattern, or a layout measured to where each flange stops and the radius begins, gives you the straight segments only. Add one bend allowance per bend: L = Σdflat + n × BA.
These are the same equation. Each outside dimension exceeds its neighbouring flat segment by exactly one setback, OSSB = tan(A/2) × (R + T), and each bend sits between two dimensions, so it adds two setbacks to the outside sum. Since BD is defined as 2 × OSSB − BA, subtracting BD from the outside sum removes those two setbacks and puts the allowance back. That identity is the best check you have: develop the same part both ways and the answers must match to the last decimal. If they do not, one of the two dimension sums was taken on the wrong basis.
Two special cases fall out. At 180° the outside faces are parallel, the setback is infinite, and the outside basis simply does not exist — a hem must be developed from flat segments. And at shallow angles with generous radii the deduction turns negative, which means the blank has to be longer than the sum of outside dimensions. Both are real geometry, not errors.
Worked example: a U-channel in 1/16 in steel
The drawing calls for a channel 4.000 in wide with 2.000 in legs, all dimensions to the outside, in 0.0625 in steel bent to a 0.0625 in inside radius. The shop has measured K = 0.42 on this tooling.
- Sum the outside dimensions. 2.000 + 4.000 + 2.000 = 8.000 in, across two bends.
- Bend allowance. R + K·T = 0.0625 + (0.42 × 0.0625) = 0.08875 in. BA = 1.5707963 × 0.08875 = 0.139396 in.
- Setback. tan(45°) = 1, so OSSB = 1 × (0.0625 + 0.0625) = 0.125 in.
- Bend deduction. BD = (2 × 0.125) − 0.139396 = 0.110604 in.
- Develop. 8.000 − (2 × 0.110604) = 7.778791 in.
Cross-check on the other basis. Each 2.000 in leg loses one setback, giving 1.875 in of flat; the 4.000 in web loses a setback at each end, giving 3.750 in. Total flat = 1.875 + 3.750 + 1.875 = 7.500 in. Add two allowances: 7.500 + (2 × 0.139396) = 7.778791 in. The two routes agree exactly, which confirms both the arithmetic and the dimension basis.
To lay out the bend lines on the blank, work from one edge: the first tangent line falls at 1.875 in, the bend occupies 0.139396 in of arc, the web flat runs to 1.875 + 0.139396 + 3.750 = 5.764396 in, and the second bend ends at 5.903791 in, leaving the final 1.875 in leg. Those are neutral-axis positions on the flat blank, which is what a laser or turret program needs for scribe lines.
Reading the result and checking it before you cut
The developed length should always be shorter than the sum of outside dimensions on ordinary bends, and the shortfall should be roughly 0.4 to 0.5 times material thickness per 90° bend for radii near one thickness. If your deduction is far outside that band, one of the inputs is wrong — most often the inside radius, because it is set by the die opening rather than the punch, or the angle, because someone entered the included angle instead of the angle turned through.
Scale is the second sanity check. On a 20-gauge part the total adjustment across four bends is under 0.15 in, which many shops would absorb in trimming. On 1/4 in plate the same four bends move the blank by nearly 1.8 in, and no amount of trimming rescues a blank cut without it. Thickness is the dominant driver, and it enters twice — once directly in the setback and once through the K-factor offset.
The blank area output is there for nesting and cost. Multiply by density to get the weight of the blank, which is what a supplier quotes against; the steel plate weight calculator does that step and also converts to pounds per square foot.
Finally, remember what this calculator assumes: all bends share one angle, one radius and one K-factor. Real parts often mix a tight 90° corner with an open 30° break. When they do, compute the allowance for each distinct bend in the bend allowance calculator and add the results by hand, rather than averaging.
Bend deduction per 90° bend, R = T, K = 0.42
| Material | Thickness (in) | Bend allowance (in) | Bend deduction (in) | Total for 4 bends (in) |
|---|---|---|---|---|
| 20 ga steel | 0.0359 | 0.08008 | 0.06352 | 0.25410 |
| 18 ga steel | 0.0478 | 0.10662 | 0.08458 | 0.33832 |
| 16 ga steel | 0.0598 | 0.13339 | 0.10581 | 0.42326 |
| 14 ga steel | 0.0747 | 0.16662 | 0.13218 | 0.52872 |
| 12 ga steel | 0.1046 | 0.23331 | 0.18509 | 0.74035 |
| 1/16 in | 0.0625 | 0.13941 | 0.11059 | 0.44237 |
| 1/8 in | 0.1250 | 0.27882 | 0.22118 | 0.88474 |
| 3/16 in | 0.1875 | 0.41822 | 0.33178 | 1.32710 |
| 1/4 in | 0.2500 | 0.55763 | 0.44237 | 1.76947 |
Only valid at 90 degrees with the inside radius equal to thickness and K = 0.42. Change any of those and recompute; the numbers do not scale across angles.
Layout mistakes that scrap blanks
- Mixing dimension bases in one sum. Two legs measured to the outside and one to a tangent line produces a blank wrong by one setback. Pick a basis, convert everything to it, then compute.
- Counting bends that do not lie along the unfold. Only bends crossed by the direction you are developing consume length in that direction. Unfold length and width separately.
- Using a nominal gauge thickness. Sheet is supplied to a tolerance, and thickness drives both the setback and the K-factor offset. Micrometer the coil.
- Taking the inside radius from the punch. In air bending the radius comes from the die opening, roughly 16% of it in mild steel. A sharp punch in a wide die still gives a large radius.
- Applying one K-factor to a part that mixes radii. K depends on the R/T ratio. A part with one tight bend and one generous bend needs two allowances, computed separately.
- Forgetting hole-to-bend distance. A hole closer to the bend line than about 2.5 times thickness plus the radius will distort. The flat pattern positions it correctly; the process still deforms it.
How this sits alongside CAD and the press brake
Every CAD system implements this same geometry. SolidWorks, Inventor and Solid Edge all let you specify K-factor, bend allowance or bend deduction per bend, and a bend table is just a lookup of the same quantities indexed by thickness and angle. When a CAD flat and a hand calculation disagree, the cause is almost always a different K-factor or a different inside radius carried in the sheet metal style — not a different formula. Comparing the two is a fast way to audit what your CAD template actually assumes.
Upstream of the layout sits the question of whether the bend can be made at all. The die you pick fixes both the achievable radius and the force, and the press brake tonnage calculator reports the radius that a given V-die produces along with the tonnage and the shortest flange the die will hold. Work in that order: choose the die, read the radius, then develop the blank. Choosing a radius first and finding no die produces it is the usual sequence error.
Downstream, the blank feeds cutting and material planning. Once you know the developed length and width, the metal weight calculator and plate weight calculator turn the blank into pounds for quoting and freight. If the part is structural rather than enclosure sheet, the strength of the formed section is a separate question — forming does not change the material, but it does work-harden the bend zone, which a tensile check on the flat material will not capture. The stress and strain calculator covers the elastic behaviour of the parent material.
One older convention is worth recognising. Aircraft sheet-metal practice often uses a setback table and a fixed bend-allowance chart rather than a K-factor, and some shops still work in the Y-factor, which equals K × π/2 and folds the radian conversion into the constant. Both encode the same neutral-axis assumption; the K-factor form simply exposes the empirical part so you can measure it.