Free Engineering Tool
Compute the flat pattern length of bent sheet-metal parts using the neutral-axis arc method with material-specific K-factors. Enter material, thickness, inside radius, bend angle and flange lengths — the calculator returns bend allowance (BA), bend deduction (BD), outside setback (OSSB) and the flat blank length for L and U shapes, plus a reverse mode to back-calculate the K-factor from measured parts.
When sheet metal bends, the outer surface stretches and the inner surface compresses. The neutral axis — the position that is neither stretched nor compressed — shifts inward from the geometric centre. The K-factor (0–1) describes that position as a fraction of thickness: K = 0.5 means the neutral axis is at the centre, while typical air-bending values are 0.3–0.4. This is the same method our engineers use when programming press brakes and generating flat patterns for laser cutting.
Geometry within recommended limits for this material.
Geometric values only — springback is not modelled. Confirm with a first-article bend; typical overbend compensation is 2–5° for mild steel, 5–10° for stainless and 5–8° for aluminium. See DIN 6935, ISO 7438 and Machinery's Handbook.
The flat pattern length is the sum of the straight flange lengths minus the bend deduction. The bend allowance is the neutral-axis arc through the bend.
Units: R and t in mm, α in degrees. Flange lengths are measured to the bend intersection (mold line), which is the convention used in CNC press-brake programs.
| Material | t (mm) | R (mm) | BA (mm) | BD (mm) | V-die (mm) |
|---|---|---|---|---|---|
| Mild Steel | 1 | 1 | 2.26 | 1.74 | 8 |
| Mild Steel | 1.6 | 1.6 | 3.62 | 2.78 | 13 |
| Mild Steel | 2 | 2 | 4.52 | 3.48 | 16 |
| Mild Steel | 3.2 | 3.2 | 7.24 | 5.56 | 26 |
| Stainless 304 | 1 | 2 | 3.85 | 2.15 | 8 |
| Stainless 304 | 1.6 | 3.2 | 6.16 | 3.44 | 13 |
| Stainless 304 | 2 | 4 | 7.7 | 4.3 | 16 |
| Stainless 304 | 3.2 | 6.4 | 12.32 | 6.88 | 26 |
| Aluminium 5052 | 1 | 1 | 2.2 | 1.8 | 8 |
| Aluminium 5052 | 1.6 | 1.6 | 3.52 | 2.88 | 13 |
| Aluminium 5052 | 2 | 2 | 4.4 | 3.6 | 16 |
| Aluminium 5052 | 3.2 | 3.2 | 7.04 | 5.76 | 26 |
| Aluminium 6061 | 1 | 1.5 | 3.02 | 1.98 | 8 |
| Aluminium 6061 | 1.6 | 2.4 | 4.83 | 3.17 | 13 |
| Aluminium 6061 | 2 | 3 | 6.03 | 3.97 | 16 |
| Aluminium 6061 | 3.2 | 4.8 | 9.65 | 6.35 | 26 |
Reference values computed for 90° bends with bottoming-style K-factors (≈ 0.44 mild steel, 0.45 stainless, 0.40–0.42 aluminium). The calculator defaults to air-bending K-factors (0.33–0.35) — enter the K-factor for your process to match your shop results. Thicknesses are common commercial sheet gauges; each row uses that material's minimum bend radius.
2 mm mild steel (K = 0.33) bent 90° with a 3 mm inside radius: BA = (π/180) × 90 × (3 + 0.33 × 2) = 5.76 mm. OSSB = (3 + 2) × tan(45°) = 5.0 mm. BD = 2 × 5.0 − 5.76 = 4.24 mm. For an L-shape with 50 mm + 30 mm legs: flat length = 50 + 30 − 4.24 = 75.76 mm.
The K-factor depends on material, thickness, bend radius and bending method. Good starting values for air bending: mild steel 0.33, stainless steel 0.35, aluminium 0.33. For bottoming (bottom bending), add 0.05–0.10. For precise results, bend a test piece, measure the flat blank and the formed legs, then use this calculator's reverse mode to back-calculate the K-factor. CNC press-brake controllers usually have built-in K-factor libraries by material.
For standard air bending, the V-die opening should be about 8 times the sheet thickness (8T). Use about 6T for thin sheet (< 1.5 mm) and 10–12T for thick plate (> 6 mm). A wider opening needs less tonnage but increases the actual inside radius and springback; a narrower opening marks the part, increases tonnage and can damage the die.
All metals spring back after bending because the elastic strain component recovers when the load is removed. Springback increases with material strength and bend radius, and decreases with thickness. Typical values: mild steel 2–5°, stainless steel 5–10°, aluminium 5–8°. Compensate by overbending by the springback amount, using bottoming or coining instead of air bending, or adjusting the angle-compensation table on the press-brake controller.
Bend allowance (BA) is the arc length of the neutral axis through the bend — the actual material consumed by the bend. Bend deduction (BD) is the amount you subtract from the sum of the flange lengths (measured to the bend intersection) to get the flat blank length. They are related by BD = 2 × OSSB − BA, where OSSB = (R + t) × tan(α/2) is the outside setback. BA tells you how much material the bend uses; BD tells you how much to take off the measured legs.
It depends on how the legs are measured. If legs are measured to the bend intersection (mold line), the two legs overlap at the corner, so you subtract BD. If legs are measured to the outside tangent points, the flat length equals legs + BA. The two methods give the same answer; this calculator follows the mold-line convention, which is what CNC press-brake programs and most drawings use.
The minimum inside radius is set by material ductility: mild steel can be bent to about 1T (one thickness), stainless steel 304 needs about 1.5–2T, and aluminium 6061-T6 about 2–3T. Bending below the minimum cracks the outer fibre. The calculator warns when the entered radius is below the recommended minimum for the selected material.
The flat-pattern length is a solid first estimate and directly affects material usage and cost. For a final production quote, send your drawing to Balford at shawn@balford.net — our engineers confirm material, K-factor, tolerances and price, typically within 24 hours.
Send your drawing to shawn@balford.net — our engineers will confirm K-factors, flat patterns and pricing within 24 hours.