- Understand flat development with the BA formula; calibrate with same-material coupons.
- Inside radius must match grade, temper, thickness and grain.
- Screen hole-edge-to-bend-tangent distance from R+2t.
- Control multi-bend parts from functional datums, not uniformly tight flanges.
Values in this guide are practical starting points for RFQ, DFM and prototype validation. They do not replace load calculations, regulations, material certificates, qualified procedures or approved production drawings.
Use the Formula to Understand—Then Calibrate
Bend allowance can be expressed as BA=(π/180)×A×(R+K×t), where A is bend angle, R inside radius, t thickness and K the neutral-axis factor. Air-bending K values often start around 0.30–0.45, but material, R/t and tooling shift the result. For critical work, bend coupons from the production material, back-calculate deduction and freeze the flat pattern.
Match Inside Radius to Grade and Temper
For a 90° bend, R≈1t is a general DFM starting point for mild steel; 304 stainless may start around 1–2t; 5052-H32 aluminum often starts near 1t, while 6061-T6 usually needs a larger radius with strong thickness dependence. Bending across the grain generally reduces cracking risk. The material supplier's minimum radius, cosmetic requirement and trial bend control.
Keep Features Out of the Bend-distortion Zone
A practical initial rule is hole edge to bend tangent ≥R+2t. Long slots, square openings and edge cutouts may need more distance or bend relief. If a functional hole must remain close, drill/ream after forming, compensate its preform geometry or add relief. Measure from the nearest hole edge, not only the center.
Reliefs and Minimum Flange
A bend relief may start at width ≥t and extend beyond roughly R+t, then be adjusted for appearance and tooling. Minimum flange depends on V-opening: air bending commonly uses V around 6–10t, with minimum flange often about 0.7V or more. Thick or hard material and larger radii need wider dies. Simulate every bend in box parts to prevent formed flanges from colliding with tooling.
Apply Tolerance to the Functional Result
±1° is a reasonable initial discussion point for ordinary bends; dedicated tooling and stable material can do better, but multiple bends and long-flange springback accumulate variation. Do not apply a single-flange tolerance blindly to a dimension across three bends. Control mounting faces, holes and envelope, relax nonfunctional flanges, and define inspection datums plus free-state or restrained condition.
DFM CHECK
- Grade, temper, thickness and rolling direction
- R/t, V-opening, K-factor and flat-pattern ownership
- Hole-to-bend distance, relief and minimum flange
- Bend sequence, tool collision and marking limits
- Trial bend and first-article record for critical geometry