A sheet metal enclosure came off the press brake with the flange 2 mm short. The drawing said the flange should be 40 mm after bending. The part measured 38 mm. The shop bent it again — same result. The laser-cut flat was right, the bend was right, the press brake was calibrated. The problem was the bend allowance used in the CAD model. The designer used the default K-factor of 0.44 for a 1.5 mm sheet with a 1.5 mm radius. For that material, the actual K-factor was closer to 0.31.
What the K-factor actually is
When a sheet bends, the material on the outside of the bend stretches and the material on the inside compresses. Somewhere in the middle there’s a neutral plane — a line that doesn’t stretch or compress. Its length equals the flat length of the part. The K-factor is the position of that neutral plane, expressed as a fraction of the material thickness from the inside surface.
K = 0.44 means the neutral plane sits at 44% of the thickness from the inner face. That’s the default in most CAD packages (SolidWorks, Inventor, and Fusion all default somewhere in the 0.4-0.5 range). The problem: the K-factor depends on the material, the bend radius, the bend angle, the direction of rolling, and the tooling. A default value is a guess that happens to work for 1.0 mm mild steel with a 1.0 mm radius. Change any of those and the flat pattern drifts.
The formula
Bend allowance (BA) is the length of the neutral plane through the bend:
BA = θ × (π/180) × (R + K × T)
where θ is the bend angle in degrees, R is the inside radius, K is the K-factor, and T is the material thickness. For a 90° bend in 1.5 mm sheet with R = 1.5 mm and K = 0.31:
BA = 90 × (π/180) × (1.5 + 0.31 × 1.5) = 1.571 × (1.5 + 0.465) = 1.571 × 1.965 = 3.09 mm
With the CAD default of K = 0.44, the same bend gives:
BA = 1.571 × (1.5 + 0.66) = 1.571 × 2.16 = 3.39 mm
The difference is 0.3 mm per bend. The enclosure flange in question had two bends. The 0.3 mm per bend accumulated to 0.6 mm — not the full 2 mm error, but the beginning of it. The rest came from the springback compensation being added on top of the already-wrong allowance.
K-factor vs. bend deduction
Press brake operators don’t think in K-factor. They think in bend deduction (BD) — how much to subtract from the sum of the outside dimensions to get the flat length. For a 90° bend:
BD = 2 × (R + T) − BA
For the 1.5 mm sheet with R = 1.5 and K = 0.31: BD = 2 × 3.0 − 3.09 = 2.91 mm. The operator’s cheat sheet says “1.5 mm sheet, 1.5 mm radius, 90° — deduct 2.9 mm.” That number comes from a bend test, not from a formula. The reliable shops have a bend deduction table per material, per thickness, per radius, developed by bending test pieces. The CAD model should use the same numbers.
Why the default fails on stainless
Stainless steel work-hardens more than mild steel. Its K-factor is lower — the neutral plane sits closer to the inside of the bend because the outer fibers resist stretching more. For 1.5 mm 304 stainless with a 1.5 mm radius, the measured K-factor is about 0.30-0.34. For aluminum 5052, it’s higher — around 0.40-0.45, because aluminum work-hardens less. Using a single K-factor across all materials is the fastest way to get wrong flat patterns.
| Material | Thickness | Radius | Measured K | BD (90°) |
|---|---|---|---|---|
| Mild steel CRS | 1.0 mm | 1.0 mm | 0.42 | 1.83 mm |
| Mild steel CRS | 1.5 mm | 1.5 mm | 0.38 | 2.91 mm |
| 304 stainless | 1.5 mm | 1.5 mm | 0.31 | 3.09 mm |
| 5052 aluminum | 1.5 mm | 1.5 mm | 0.44 | 2.71 mm |
| Mild steel | 2.0 mm | 1.0 mm (sharp) | 0.32 | 4.16 mm |
The 304 stainless enclosure had a default K of 0.44 applied to it. The actual was 0.31. Every flange came out short by 0.3 mm per bend. The designer changed the K-factor in the CAD model to 0.31, regenerated the flat patterns, and the parts came off the brake within 0.1 mm.
The bend test that settles it
Any shop that does serious sheet metal work should run a bend test on each material/thickness combo it uses. Cut a strip 100 mm x 30 mm, bend it 90° with the production tooling, measure the outside dimensions, and back-calculate the K-factor. It takes 10 minutes per material. The result is a table the CAD department uses instead of the default. This is the difference between a shop that reworks 15% of its parts and one that reworks 2%.
The test strip method: after bending, measure the two legs (L1, L2) from the outside. The flat length was 100 mm. The bend deduction BD = L1 + L2 − 100. Then K = (2 × (R + T) − BD) / (1.571 × T) − R/T… — the exact algebra doesn’t matter for the shop floor. What matters is the BD lands in a table, gets used, and gets verified on the next batch.
Springback is a separate problem
Bend allowance gets the flat length right. Springback gets the bend angle right. The press brake over-bends by the springback amount — for stainless, that’s 2-5° at a 90° bend with a 1.5 mm radius. The operator compensates by over-bending the top dead center or using the CNC program’s bend compensation. If the flat is wrong AND the springback compensation is applied, the errors stack. Fix the flat first, then tune the angle.
The enclosure’s 2 mm error was mostly the K-factor. But the operator had also been adding 1° of over-bend to compensate for springback — the two corrections fought each other. Once the flat pattern was right, the over-bend was set to the true springback value and the parts dropped in tolerance.
The default K-factor is a starting point, not a design value. Run a bend test per material and thickness, put the bend deduction in a table, and use it in the CAD model. The 2 mm short flange wasn’t the press brake — it was 0.3 mm of wrong allowance per bend, on two bends, on stainless. Measure once, bend a test strip, and the flat pattern stops lying.
