A sheet metal enclosure that came out 4 mm short. The fabricator cut the flat pattern from the 3D model, bent it on a press brake, and the side panels didn’t meet. The designer had used the default bend allowance in the CAD software — the one that’s pre-programmed and works for mild steel at 90 degrees with an air-bent V die. The part was aluminum, 2 mm thick, bent to 120 degrees. The default value was wrong for both.

What bend allowance actually is

When a sheet metal part is bent, the inside radius compresses and the outside stretches. Somewhere between them is the neutral axis — the plane that doesn’t change length. The bend allowance (BA) is the length of the neutral axis through the bend. The flat pattern length is the sum of the straight sections plus the bend allowances. Get the BA wrong and every bend on the part is off by the same amount.

The rule of thumb for a 90-degree air bend in mild steel: BA = 0.45 × thickness, per bend, for an inside radius equal to the thickness. That’s the default in most CAD packages. It works for that one case. For a 2 mm aluminum part bent to 120 degrees with an inside radius of 1 mm, the default is wrong.

The formula that works for any angle

The K-factor method is the standard. K is the ratio of the neutral axis position to the thickness. For air bending, K typically runs 0.33 to 0.50. The bend allowance is:

BA = π × (R + K × T) × (A / 180)

Where R is the inside radius, T is the thickness, A is the bend angle in degrees.

For the failing part: R = 1 mm, T = 2 mm, A = 120°, K = 0.44 (for aluminum, air-bent).

BA = π × (1 + 0.44 × 2) × (120 / 180) = π × 1.88 × 0.667 = 3.94 mm

The CAD default used K = 0.33 (a steel value) with R = 1 mm:

BA_default = π × (1 + 0.33 × 2) × 0.667 = π × 1.66 × 0.667 = 3.48 mm

The difference is 0.46 mm per bend. The enclosure had four bends per panel. The flat pattern was short by 1.84 mm per panel. The 4 mm total gap on the enclosure was four panels × 0.46 mm × 2 ends. The math checks out.

The K-factor depends on the process, not just the material

Air bending (the punch pushes the material into a V die without bottoming) has a different K-factor than bottoming (the punch forces the material to the die bottom) or coining (the material is squeezed to full die depth).

  • Air bending, R ≈ T: K = 0.44 (aluminum), 0.38-0.42 (mild steel)
  • Bottoming, R ≈ 0.5T: K = 0.33-0.35
  • Coining, R ≈ 0: K = 0.30-0.33

The CAD default of 0.33 is a bottoming/coining value. If your shop air-bends (most do), the flat pattern will be short. The fabricator had been compensating with a fudge factor — they added 0.5 mm per bend by hand. When the designer switched to a new CAD version, the compensation was lost and the parts came out short.

Why 120 degrees breaks the simple rule

The 0.45 × T rule of thumb is only valid for 90 degrees. At 120 degrees, the neutral axis moves toward the inside (K drops slightly), and the simple linear rule overestimates the allowance. The error grows as the angle deviates from 90. A 45-degree bend with the 90-degree rule is off by 10%. A 135-degree bend is off by 8%. If your parts have mixed angles, calculate each bend with the full formula, or better, use the bend table in your CAD package that’s set to your actual tooling.

The fix in practice

The enclosure flat patterns were regenerated with K = 0.44 and the full angle formula. The parts fit on the first try. The fabricator also updated the CAD bend table to match their press brake tooling — they ran a test bend, measured the neutral axis position, and set the K-factor from real data instead of a book value.

The test bend procedure: cut a 100 mm strip, bend it 90 degrees, measure the outside dimensions, and back-calculate the K-factor. It takes 10 minutes and it calibrates the software to the actual tooling. Every shop with a press brake should do it once per material and thickness. The result: no more short parts, no more fudge factors, no more scrap.

The springback question

Springback is the other variable. After the bend, the material springs back a few degrees. The punch over-bends to compensate. Springback is higher for aluminum (about 2-3 degrees for 90-degree bends in 2 mm) and higher for harder materials. The CAD model should be checked against the actual part — if the angle comes out 88 degrees instead of 90, the punch angle needs to be 2 degrees more. Springback is a die setup variable, not a flat pattern variable. It doesn’t affect the BA — it affects the angle. Keep the two separate in your head, and the parts will come out right.

Bend allowance is a calculation, not a default. Use the K-factor formula with the angle, material, and process-specific K. Calibrate the K-factor from a test bend, and check springback as a die setup item. The enclosure that came up 4 mm short wasn’t a CAD bug — it was a steel K-factor applied to aluminum, and a 90-degree rule applied to 120-degree bends.