Sheet Metal Bending Calculator

How Is Sheet Metal Bend Allowance Calculated?

When sheet metal is bent, the outer surface stretches and the inner surface compresses. The neutral axis — where no stretching or compression occurs — shifts inward from the geometric center. The K-factor (0 to 1) describes the neutral axis position as a ratio of thickness: K = 0.5 means the neutral axis is at the center, while this calculator's own air-bending defaults range 0.40-0.45 by material.

Bend allowance (BA) is the arc length of the neutral axis through the bend, representing the amount of material consumed by the bend. Bend deduction (BD) is the difference between the sum of flange lengths (measured to the bend intersection) and the flat pattern length. These values are essential for accurate flat pattern development in CNC programming.

The V-die opening typically follows the 8T rule (die opening = 8 × material thickness) for standard bending. The minimum bend radius is not a single multiple of thickness. For steel, DIN 6935 tabulates it by thickness band, tensile strength class and bend orientation: the effective multiple runs from 1T in thin sheet to about 2T in ordinary plate, and a bend along the rolling direction needs a larger radius than one across it. This calculator reads that table for mild steel; the alloys have no equivalent sourced table and fall back to conventional shop multiples, and the result says which of the two it used. Going below the minimum radius causes cracking on the outer surface.

Formula: BA = (π/180) × Bend Angle × (Inside Radius + K × Thickness) BD = 2 × (Inside Radius + Thickness) × tan(Angle/2) − BA Flat Length = Leg1 + Leg2 − BD (L-shape) K-factor = t/T (neutral axis offset / thickness)

Example Calculation

Bending 2 mm mild steel (K=0.44) at 90° with 3 mm inside radius: BA = (π/180) × 90 × (3 + 0.44 × 2) = 6.09 mm. OSSB = (3 + 2) × tan(45°) = 5.0 mm. BD = 2 × 5.0 − 6.09 = 3.91 mm. For a 50 mm + 30 mm L-shape: Flat length = 50 + 30 − 3.91 = 76.09 mm.

When to Use This Calculator

• Developing flat patterns for CNC laser/plasma cutting — accurate bend deduction is critical for parts that fold up to the correct dimensions
• Programming a CNC press brake and needing the correct bend allowance for the tooling setup and material combination
• Reverse-engineering an existing bent part — measuring the formed part and calculating the K-factor for future production
• Quoting sheet metal fabrication jobs — accurate flat pattern length determines material usage and cost
• Selecting the appropriate V-die opening for a given material thickness and inside bend radius

Common Mistakes to Avoid

• Using a generic K-factor (0.5) instead of the material-specific value — this calculator's default for mild steel is K=0.44, not 0.5; the wrong K-factor produces flat patterns with error that compounds on parts with multiple bends
• Measuring flange length to the outside of the bend instead of to the bend intersection — the formula requires dimensions measured to the mold line (theoretical sharp corner)
• Forgetting that the inside radius is controlled by the V-die opening (not by the punch radius) in air bending — the actual inside radius ≈ V-die opening × 0.156 for standard tooling
• Ignoring springback — all materials spring back after bending; stainless steel springs back 3-5° more than mild steel, requiring overbend compensation
• Bending parallel to the rolling direction on aluminum — this causes cracking at the outer fiber; always orient bends perpendicular to the grain direction

How to Interpret Results

• Flat pattern length (or bend deduction) drives the blank size — BD is subtracted from the sum of flange lengths measured to the mold line, and an error here repeats on every bend in the part
• The K-factor shown is the value actually used in the calculation — validate it with a test coupon for new material/tooling combinations, using the K-factor reverse mode to back-calculate from measurements
• If your inside radius is below the minimum bend radius output, expect outer-fiber cracking — increase the radius or orient the bend across the rolling direction; heed any warnings the calculator raises
• The recommended V-die follows the 8T rule — a narrower die raises tonnage and marks the part, while a wider die increases the actual inside radius and springback
• Springback is not modeled — the results are purely geometric; verify the first article and apply overbend compensation (typically 2-5° for mild steel, 5-10° for stainless) at the press brake

Related Standards & References

• DIN 6935 — Cold bending of flat steel products (source of the minimum bend radius table used here; steel only, no aluminium alloys)
• ISO 7438 — Metallic materials — Bend test (test method; it sets no minimum bend radius, leaving the former diameter to the product standard)
• ASME Y14.5 — Dimensioning and tolerancing (for specifying bent part dimensions on drawings)
• Machinery's Handbook — general bend allowance and K-factor background

Bend Allowance Reference — 90° Bends

All dimensions are in millimetres. Figures are computed by this calculator. Each row bends at that material's minimum bend radius. Thicknesses are commonly stocked sheet sizes, not a normative series.

Frequently Asked Questions

How do I determine the correct K-factor for my material?

K-factor depends on material, thickness, bend radius, and bending method. This calculator's own air-bending defaults are: mild steel 0.44, stainless 304 0.45, aluminum 5052 0.40, aluminum 6061 0.42. Bottoming — add 0.05-0.10 to these values. For accurate results, bend a test coupon, measure the flat pattern versus formed dimensions, and back-calculate K. CNC press brake controllers often have material-specific K-factor libraries.

What is the 8T rule for V-die selection?

The V-die opening should be approximately 8 times the material thickness (8T) for standard air bending. For thinner material (<1.5 mm), use 6T; for thicker material (>6 mm), use 10-12T. A wider die opening reduces required tonnage but increases minimum bend radius and springback. Too narrow a die opening causes marking, excessive tonnage, and potential die damage.

How does springback affect bend accuracy and how do I compensate for it?

All metals spring back after bending because the elastic strain component recovers when the bending force is removed. Springback increases with higher material strength, larger bend radius, and thinner material. Typical values: mild steel 2-5°, stainless steel 5-10°, aluminum 5-8°. Compensation methods: overbend by the springback angle, use bottoming or coining instead of air bending, or adjust the press brake controller's angle correction tables.