Bend reliefs

Purpose and scope

A bend-end relief separates material that must move during forming from adjacent stock.

Bounded fabricator example: SendCutSend recommends relief width at least half material thickness and depth at least thickness + bend radius + 0.020 inch, measured from its stated bend line. For assumed thickness 0.100 inch and radius 0.060 inch, the calculation gives width 0.050 inch minimum and depth 0.180 inch minimum under that guidance. These inputs are illustrative, not a selected material/tooling combination or a general manufacturing approval. SendCutSend sizing and reference diagram

Protolabs' August 15, 2022 bend-relief article explains the separation of bent and unbent elements and its use to avoid deformation during press-brake forming. This is fabricator guidance, not a universal dimensional standard or a guarantee that adding a notch prevents every failure. Protolabs, how and when to add bend reliefs

Define the intended result first: clear forming movement, a controlled flange junction, an accessible tool path or a specified corner gap. Reliefs do not replace the checks for material ductility, bend radius, flange length, tooling and final structural function.

Where a relief belongs

Check both ends of each local bend and the intersection of adjacent flanges. The relevant question is whether neighboring material remains connected across a region that must deform differently. A full-width bend ending at free edges is different from a short flange beside an unbent tab.

SendCutSend's January 18, 2024 guide illustrates bends needing two, one or no reliefs. It distinguishes ordinary bend-end relief from corner relief and uses its own air-bending material/tooling data for effective bend radius. Do not apply a relief everywhere merely because the model contains a bend. SendCutSend bend-relief guide

Inspect the flat pattern and formed model together. In the flat state, verify that the cut removes the intended material; in the formed state, check separation, remaining stock, flange interference and access for subsequent operations. A cut that looks adequate from one view can leave a small remnant or an unwanted opening in another.

Geometry and dimensional references

“Relief depth” is especially ambiguous without its reference. A dimension from a flat-pattern bend line is not automatically the same as a CAD parameter measured beyond the bend region. Preserve the diagram or explicit datum with the number.

Protolabs' cited article instead discusses a cutout at least 0.030 inch wide and extending at least 0.015 inch beyond the end of the bend radius. The numerical recipe and reference differ. Use the chosen fabricator's reviewed layout rather than blending guidance from different services. Protolabs bend-relief dimensions

A larger cut is not automatically better. Review removed material against load paths, mounting positions, appearance, sealing and permitted openings. If a relief intersects another hole or slot, the resulting geometry requires evaluation as a combined feature.

CAD reliefs represent geometry rules

SOLIDWORKS 2026 Help supports rectangular, tear and obround automatic reliefs. Its relief-ratio relation is d = relief ratio × part thickness, where d describes cut width and the extension beyond the bend region shown in its diagram. The permitted software ratio range is 0.05–2.0. That is a CAD input range, not a validated fabrication window. SOLIDWORKS 2026, Auto Reliefs

For an illustrative 2.0 mm model thickness and ratio 0.5, d = 1.0 mm. This does not mean the total notch depth is 1.0 mm from an arbitrary bend-center line. Check the help diagram and the actual generated flat pattern before transferring the value to a drawing.

Autodesk Fusion separately controls relief shape, width, depth and remnant, and distinguishes bend relief from two- and three-bend corner relief. Its reference defines remnant as the minimum stock alongside the relief cut and gives separate corner placement options. The live help page has no independently verified release date. Autodesk Fusion sheet-metal rule reference

Do not equate similarly named parameters across CAD systems without comparing their geometric definitions. Record the rule and feature overrides used, then inspect the exported geometry. A model that unfolds successfully demonstrates software geometry, not acceptable forming, strength or surface quality.

Tear relief and controlled edges

SOLIDWORKS describes tear relief as the minimum geometry needed to insert a bend and flatten the part, with Rip and Extend options. Fusion describes its tear option as creating no cut relief so material tears at the corner. These are software-specific behaviors; the shared label does not establish an acceptable physical edge for the application. SOLIDWORKS Auto Reliefs, Fusion relief reference

When a controlled cut and edge condition are required, specify them explicitly rather than relying on an unexplained tear setting. Agree burr orientation, deburring, cut-end shape and any prohibited cracking with the fabricator. Avoid assigning a universal fatigue benefit to a particular relief shape without evidence for the actual component.

Manufacturing review and acceptance

Review reliefs against the complete process: cutting, forming sequence, tooling access, joining and finish. Where a corner must be sealed or cosmetically closed, establish the joining/finishing requirement separately; the relief itself creates clearance rather than proving a sealed joint.

A practical review sequence is:

1. Identify material/condition, thickness, bend process and effective radius.
2. Mark the bend region, reference line and relief geometry in the flat pattern.
3. Verify formed clearance, remaining material and neighboring features.
4. Obtain fabricator acceptance of cutting limits, tooling and forming sequence.
5. Inspect the finished corner for agreed dimensions, deformation and edge condition.

For agent-readable records, store rule source/version, shape, dimensions, units and measurement references alongside the material and bend parameters. Keep a fabricator recommendation, a CAD default and a contractual acceptance limit distinguishable. Recheck the relief when thickness, radius, flange layout or manufacturing route changes.