A batch of 100 brackets came off the press brake 2 mm short on the critical dimension. The drawing said 100 mm overall, and the parts measured 98 mm. The shop checked the tooling, the material, and the press. The CAD model’s flat pattern was wrong. The K-factor the software used didn’t match the actual material and the air bend radius. This happens on every sheet metal part where nobody verifies the K-factor.

The flat pattern math

A bent sheet has a neutral axis, the plane inside the material that neither stretches nor compresses. The flat length equals the sum of the straight segments plus the bend allowance, the arc length along the neutral axis.

The K-factor is the ratio of the neutral axis position to the material thickness. K = 0.5 means the neutral axis sits at the center. For a sharp bend, the neutral axis shifts inward and K drops to about 0.33. For a large radius bend, K approaches 0.5.

The CAD default for mild steel is usually 0.44. The bracket used 1.5 mm mild steel bent at 90 degrees with an air bend radius of 1.5 mm (R/T = 1.0). For that ratio, the actual K is about 0.35. The default 0.44 overestimated the bend allowance by about 1 mm per bend. Two bends, 2 mm short. Exactly what the shop measured.

The formula and the worked example

Bend allowance BA = angle x (pi/180) x (R + K x T), where angle is the bend angle, R is the inside radius, and T is the thickness.

For the bracket: 90 degrees, R = 1.5, T = 1.5, K = 0.35. BA = 90 x 0.01745 x (1.5 + 0.35 x 1.5) = 1.5708 x 2.025 = 3.18 mm.

With the CAD default K = 0.44: BA = 1.5708 x (1.5 + 0.66) = 1.5708 x 2.16 = 3.39 mm. The difference is 0.21 mm per bend, 0.42 mm total for two bends. That’s not the 2 mm the shop measured. The rest came from the air bend radius being larger than nominal.

Air bending with a V die produces an inside radius of about 0.15 to 0.2 of the die width, not the nominal radius in the drawing. For a 12 mm V die on 1.5 mm steel, the actual radius is about 1.8 mm, not 1.5. Recalculating with R = 1.8 and K = 0.38 (R/T = 1.2): BA = 1.5708 x (1.8 + 0.57) = 1.5708 x 2.37 = 3.72 mm. The default gave 3.39 mm, a difference of 0.33 mm per bend, 0.66 mm total. Still not 2 mm.

The remaining error: the shop’s bend deduction method. If the press brake operator uses a bend deduction table based on the die, not the drawing, the flat pattern carries a third source of error. The fix is to build the flat pattern from a bend deduction measured on the actual tooling, not assumed from the CAD.

The K-factor by material

Mild steel, air bend: K = 0.33 to 0.44 depending on R/T. For R/T = 1.0, K is about 0.35. For R/T = 2.0, about 0.42.

Stainless 304: about 0.35 to 0.42, slightly lower because it work-hardens and springs back more. Springback makes the actual angle smaller than the die, and the operator compensates with a shallower bend angle, which shifts the neutral axis.

Aluminum 5052: K around 0.40 to 0.45, higher because it’s softer. Aluminum also springs back less, so the bend angle is closer to the die.

Use a K-factor table, not the default. If the part is critical, cut a test strip, bend it, measure the flat length, and back-calculate the K-factor for that material and tooling. It takes 20 minutes and eliminates the 2 mm short parts.

The DFM rules that prevent the phone call

Minimum bend radius: mild steel about 0.5-1x T, stainless 1-2x T, aluminum 1-1.5x T. Tighter than that cracks the outside fiber.

Minimum flange length: about 4x T + R, or the flange won’t reach over the die.

Hole-to-edge distance: a hole near a bend distorts. Keep the hole edge at least 2x T + R from the bend line, or the hole becomes oval.

Hole diameter vs thickness: holes smaller than T punch poorly, the punch breaks. For thin material, holes under 1 mm are unreliable.

Springback: the part that never matches the drawing

Air bending springs back. 90 degrees in the die comes out at 92-94 degrees in mild steel. The operator over-bends by the springback angle. That over-bend also moves the neutral axis, changing the flat length by a fraction. On critical parts, build the flat pattern from the springback-compensated angle, not the drawing angle. Most shops just over-bend and measure, which works until a new operator uses a new die.

The 2 mm short brackets weren’t a press problem. The CAD K-factor default of 0.44 didn’t match the actual material and die at 0.35-0.38. Cut a test strip, measure the bend allowance, and build the flat pattern from the real tooling. The 20-minute test saves a 100-part scrap batch.