Corner reliefs
Process-specific cutouts that provide clearance at sheet-metal bend intersections or machined internal corners.
Tags: parts-and-design, features, manufacturability
On this page
Sheet-metal corner relief frees interacting bend regions. Machined corner relief clears material left by a rotating cutter. Specify which operation and interference the cut addresses.
Supplier table plus original arithmetic: SendCutSend's bending calculator lists 0.063-inch 5052 aluminum with a 0.035-inch effective radius at 90°, 0.118-inch bend relief depth and 0.030-inch minimum corner-relief distance from the bend line. These last two columns describe different quantities. SendCutSend, Bending Calculator
Identify the manufacturing problem
| Feature | Intended function | Important design inputs |
|---|---|---|
| Sheet-metal bend-end relief | Separate bending material from adjacent flat stock | Thickness, bend radius, bend extent and cutting process |
| Sheet-metal corner relief | Accommodate intersecting bends at a tray or box corner | Flange layout, bend sequence, gap and seam requirements |
| Machined internal-corner relief | Allow a mating component to seat despite cutter radius | Cutter access, pocket depth, mating profile and remaining wall |
SendCutSend distinguishes a bend relief at a single bend beside flat material from a corner relief where two or three bends meet. Its explanation describes removal that both separates neighboring regions and provides space for deformation. Not every bend needs a separate notch: an end that reaches a free edge differs from a bend that stops within surrounding material. SendCutSend, relief design guide, 18 January 2024
The first design question is therefore where material must move or where a tool must reach. Adding identical holes to every visible corner can remove useful material without solving the actual interference.
Sheet-metal geometry and reference points
Protolabs explains that an unrelieved transition can pull adjacent material into the bend, causing deformation or tearing. Its guidance favors round reliefs over square-ended cuts for reducing tear and crack propagation. This supports attention to the relief end shape; it does not establish a fatigue rating or prove that a relieved component is stronger under every load. Nearby holes can also behave as unintended reliefs and become distorted. Protolabs, How and When to Add Bend Reliefs, 15 August 2022
Dimension the relief in the flat pattern with an unambiguous origin. Identify whether a depth is measured from a bend centerline, a bend tangent/start, or an external edge. Also distinguish notch width from flange-to-flange gap and corner offset. A numerical value copied into a differently defined CAD parameter can produce a different cutout.
For its own air-bending service, SendCutSend gives a minimum relief width of half material thickness and a depth of thickness plus bend radius plus 0.020 inch, measured from the bend line. The same guide notes that Fusion and SOLIDWORKS relief-depth settings measure from the start of the bend. Treat the supplier diagram, flat pattern and software parameter definition together; do not transfer the formula blindly into a same-named field. SendCutSend, relief design guide
These are service-specific starting dimensions. Material ductility, selected tooling, cut-feature capability and the intended corner closure remain relevant. A relief that clears the bend can still violate another requirement, such as minimum ligament, sealing surface or acceptable visible opening.
CAD settings do not qualify the process
Autodesk Fusion separates ordinary bend relief from two-bend and three-bend corner relief. Its two-bend round/square relief size is measured in the unfolded body; round placement can be tangent or centered at the intersection. Its three-bend relief shape is only visible in the flat pattern. Autodesk also describes the Tear option as creating no bend relief and allowing tearing at the corner. That option is not evidence that a physical zero-width cut will be manufactured. Autodesk, Sheet metal rule reference
Inspect both folded and flat representations after changing thickness, radius or flange layout. Check local feature overrides as well as the active rule. A successful CAD rebuild establishes geometric consistency within the model; it does not demonstrate tool clearance, acceptable cracking, or a qualified welded seam.
If the corner will be welded or sealed, specify the required final condition separately from the blank cutout. Protolabs notes that it can weld a corner to provide a sealed seam when requested. That is a secondary operation requiring agreement, not an automatic property of a corner relief. Protolabs, Sheet Metal Bend Radius Guidelines
Bounded sheet-metal example
Using the supplier's depth expression, 0.063 + 0.035 + 0.020 = 0.118 inch, matching the table. Its width expression gives 0.063 / 2 = 0.0315 inch. The conversion of that calculated depth is 0.118 × 25.4 = 2.9972 mm. This reconciles one published material/thickness combination; it is not a prescription for another shop's tooling or a complete two-bend corner layout. Retain the inch-based calculation rather than substituting a rounded metric clearance into an otherwise inch-based table.
Before release, locate the actual cut boundary relative to both bends and verify the finished flange gap. A single relief-depth number cannot specify that whole intersection.
Machined pocket reliefs
A rotating end mill leaves an internal corner radius in the plane of the cut. Protolabs describes U- or C-shaped corner clearances as an alternative to using a very small end mill to approach a sharp corner. Removing extra material locally can let a square mating item fit while allowing a larger cutter and deeper access. Its published tool-size/depth examples describe its particular process, rather than a universal machining capability. Protolabs, How to Reduce CNC Machining Costs
Choose the clearance around the actual mating envelope. Check insertion direction, mating corner chamfer/radius, dimensional tolerances and coating allowance. Where a dogbone or similar overcut is acceptable, show its complete boundary and depth; do not simply label the pocket “square.” Where extra removal would intersect a fastener, thin wall or sealing land, consider changing the mating part or agreeing another manufacturing route.
A relief at the vertical wall intersection does not automatically clear the pocket floor-to-wall fillet. Confirm the three-dimensional interface, including the required seating face. A shallow clearance that works in a top view may still leave interference lower in the pocket.
Drawing and acceptance information
Keep the release record explicit:
- Identify the relief's function and manufacturing process.
- Dimension its location, shape, depth and remaining material from named references.
- State material/thickness or pocket depth and the required final assembly condition.
- Resolve conflicts between model, flat pattern and drawing before cutting.
- Inspect critical clearances and agreed edge condition on the finished part, not solely the blank.
Specify allowable burrs or edge breaks where they affect fit and handling. For load-bearing corners, evaluate the actual remaining section and local stress concentration instead of assuming that any rounded cutout is acceptable. A first article can verify the intended forming and assembly behavior when the process has not been demonstrated.
Source scope
The SendCutSend guide displays 18 January 2024; the Protolabs bend-relief article displays 15 August 2022. The calculator, Autodesk help and other cited Protolabs design pages do not state a technical revision edition. Their guidance is used within the stated service or software context, not as a general dimensional standard.