Sheet Metal Bend Design: Radius, Flat Patterns and Formed-Part Acceptance

Key decisions

• Specify the required formed geometry and identify who owns the production flat pattern.
• Bend radius, allowance and springback depend on material and tooling conditions.
• Check nearby holes, bend relief and tool access before releasing the enclosure or bracket.

Begin with the finished bracket

A flat laser-cut blank may match its drawing perfectly and still produce an incorrect bracket after bending. The problem often begins with unclear dimension references: a flange may be measured to an outside virtual intersection in one file and to a bend tangent in another. A second source of disagreement is whether the flat pattern is a mandatory production definition or an informative export from a preliminary CAD model.

Provide a formed model and drawing that identify functional faces, angles and hole relationships. State whether the supplier may develop the blank to achieve that formed geometry. Avoid providing both an immutable blank and an incompatible formed dimension without defining which requirement governs.

Air bending and bottom bending do not use the same assumptions

TRUMPF describes air bending as a process in which punch travel produces the angle while the sheet does not fully contact the die walls. In bottom bending, the workpiece is pressed into the matching tools. These differences affect how tooling and process variables influence the result. A punch radius in a tool library should not automatically be treated as the exact final inside radius for every material and method.

SSAB identifies material properties, thickness, tool setup and other conditions as influences on final angle and radius. Therefore, changing alloy, temper or thickness can invalidate a previously useful flat pattern. The supplier needs to select a feasible tool arrangement and compensate for springback under the actual conditions. The designer should specify the finished function and any constraints on the manufacturing method, rather than assume a universal bend recipe.

Review the details that change bending feasibility

Each item below connects a drawing decision with a practical manufacturing check. The required clearance or radius must be agreed for the chosen stock and toolset. A familiar rule of thumb can be useful for preliminary layout, but it should not become an unexplained acceptance requirement.

Distinguish bend allowance from bend deduction

Bend allowance is the developed length assigned to the curved bend region. In a simple constant-radius model, BA = θ × (R + Kt), where θ is the bend rotation in radians, R is inside radius, t is sheet thickness, and K locates the neutral axis as a fraction of thickness from the inside surface. K is a process-dependent input; choosing a value in CAD does not prove it matches production.

Bend deduction is used when starting from dimensions to virtual sharp intersections rather than tangent lengths. Mixing those two conventions can count the curved region incorrectly. For non-right-angle bends, also distinguish the drawing’s included angle from the actual rotation used in the formula. The purpose of the calculation is to make assumptions visible, then calibrate them with the selected material and process.

Hole placement must survive forming

A hole that overlaps a plastically deformed region may change shape or position during bending. The required distance depends on the bend and feature geometry, sheet and tooling. When the hole is an assembly datum or close fit, ask whether it should move farther from the bend, be produced after forming, or receive a different tolerance strategy. Each option changes cost or design and requires approval.

At the end of a bend, relief can provide space for material movement and prevent an unintended tear or bulge. Its shape must also work with adjacent flanges and the finished assembly. A large relief may solve forming but leave a gap that compromises appearance, ingress protection or stiffness. Review the corner as a finished feature, including any later weld, sealant or cover.

Model tool access and accumulated variation

A box with several return flanges may be geometrically valid yet difficult to form using a particular tool arrangement. Earlier bends can block the punch, prevent a flange from entering the die or trap the part during removal. Include the full formed geometry in the RFQ so the supplier can assess sequence and tooling rather than quote only a flat outline.

A hole-to-hole relationship across multiple bends includes more sources of variation than a pattern on one untouched face. Reference dimensions from functional formed datums where appropriate. If the assembly needs adjustment, a slot can sometimes accommodate variation, but its direction and clearance must be chosen by the designer. A manufacturing proposal to add a slot should not silently change an interface that carries load or locates the assembly.

Inspect after the operations that determine function

Welding, hardware installation and finishing may alter the final component or its interfaces. A coating can change a clearance hole, and an inserted fastener can distort a thin face. State which dimensions are accepted in the final condition and where masking or protection is required. The inspection fixture should represent the drawing’s datum scheme instead of forcing a flexible bracket into an arbitrary shape.

For Beigain’s sheet-metal review, identify the alloy and condition, sheet thickness, finished model, critical dimensions and appearance requirements. A bent-part quotation should describe the offered route and any drawing assumptions. It should not rely on a generic material label or an unvalidated CAD flat pattern.

• Keep the formed drawing, model and flat pattern at one revision.
• Identify governing geometry and ownership of bend development.
• Mark hole locations, minimum clearances and critical angles in the formed state.
• State allowable relief, witness marks and surface protection.
• Include hardware, welds, finish, inspection and packaging in the same scope.

Questions about this topic

Technical references

• TRUMPF: Bending processes and methods — Machine-manufacturer explanation of air bending, bottom bending and other methods.
• SSAB: 20 questions about bending — Steel-maker guidance on material, tooling, springback and bend-radius dependencies.

Continue reading

• Sheet Metal Fabrication & Stamping
• Surface Finishing Services
• Preparing a CNC RFQ that suppliers can quote accurately
• Request a Manufacturing Quote