What is a bend relief and why does it prevent tearing?
- Share
- Issue Time
- Oct 19,2026
The short answer
A bend relief is a small notch cut at the end of a bend line, where the bend meets an edge or another flange. Without it the material has nowhere to flow, so it tears or bulges. Cut it at least one material thickness wide and as deep as the bend radius plus one thickness.
Why a bend with no relief tears
When sheet metal is formed, the outside of the bend stretches and the inside compresses, so material has to move along the bend line to accommodate the change. Where that line ends at the edge of the sheet, at a notch, or at another flange that is already formed, the material has no direction left to flow in. The strain then concentrates at the very end of the bend line: the outer fibre exceeds what the sheet can take and the corner tears, or the material piles up and bulges outwards instead. The failure is created in the flat pattern, not at the press brake, which is why a design that looks perfect in a 3D model can arrive as a box with exploded corners, sharp burrs and a deformed adjacent flange. Cutting a small piece of material away before forming gives the bend somewhere to go; that cut is the relief.
The two rules that size a relief
Two dimensions matter, and both are tied to the material thickness and the inside radius rather than to a fixed number. The relief must be at least one material thickness wide, with about twice the thickness a comfortable working value. It must be at least as deep as the bend radius plus one thickness, and roughly the bend radius plus 1.2 times the thickness if you want margin. The depth rule has a physical reason: the relief has to reach past the bend line, because a cut that stops short of it leaves the flange to tear exactly as it would with no relief at all. A worked example is easier than the algebra. For a 2 mm aluminium part with a 2 mm inside radius, the minimum relief is 2 mm wide and 4 mm deep, and 4 mm wide is the value that gives the tooling room and leaves a visibly deliberate notch rather than a ragged corner.
| Feature | Rule | For a 2 mm part, R2 |
|---|---|---|
| Relief width, minimum | 1 x material thickness | 2 mm |
| Relief width, recommended | about 2 x material thickness | 4 mm |
| Relief depth, minimum | bend radius + material thickness | 4 mm |
| Relief depth, recommended | bend radius + 1.2 x thickness | 4.4 mm |
| Minimum flange length to form | 4 x thickness + bend radius | 10 mm |
| Feature to bend distance | 2.5 x thickness + bend radius | 7 mm |
| Minimum inside bend radius | 1 x thickness, soft alloys | 2 mm |
| Minimum inside bend radius | 1.5 to 2 x thickness, hard tempers | 3 to 4 mm |
Three relief shapes and when to use each
A rectangular notch is the standard choice for laser-cut and punched work: it removes material cleanly, produces no burr, is trivial to program, and the only cost is a visible gap in the corner of the finished part. A tear relief removes nothing at all, simply slitting the corner so the metal tears along the slit as it bends; it gives the tightest corner with no visible gap, which suits a punched part where the corner will be hidden or welded, but the torn edge is jagged and sharp and can cut fingers or wire harnesses. An obround or rounded slot is the choice for parts that will see vibration or repeated load, because the rounded end spreads the stress concentration instead of leaving a sharp inside corner for a crack to start from; it is slightly slower to cut in thick material and needs the flat pattern checked. Whichever you choose, generate reliefs with the sheet-metal tool in the CAD system rather than drawing them by hand, so the geometry stays consistent with the thickness and radius actually in use.
Relief against the other rules near a bend
A bend relief is not a substitute for the rest of the sheet-metal spacing rules, and it is often confused with them. Holes and slots must sit clear of the bend line, generally at least 2.5 times the material thickness plus the bend radius away, with about 3 times the thickness as a safer figure for critical features; too close and the hole distorts into an oval as the material flows. Flanges have to be long enough for the press brake to grip them: about four thicknesses plus the bend radius is the minimum that forms consistently, and anything shorter needs special tooling or a secondary operation. The inside bend radius itself should be at least one thickness for mild steel and one and a half to two thicknesses for stainless and hard tempers, or the outer fibre cracks regardless of how good the relief is. In other words, a relief protects the end of a bend line; it does nothing for a hole placed too near the middle of one.
What a missing relief costs downstream
The immediate symptom is a torn corner and a burr that has to be dressed by hand, which is a cost in labour and a visible quality defect on any enclosure that a customer will handle. The second symptom is quieter and worse: material bulging outwards at the bend radius means the flange face is no longer flat. A lid or a mating panel then rocks on the corner bulges instead of seating, fasteners pull the joint down and distort the panel, and what looked like an assembly problem turns out to be a forming problem. The third symptom appears later, when a sharp unrelieved inside corner acts as a stress raiser and a crack begins under vibration or thermal cycling; a rounded relief changes that corner into a smooth transition and removes the initiation site. All three are avoided by a cut that takes less than a second on a laser.
How to specify it on the drawing
Show the relief on the flat pattern rather than describing it in a note, because that is the drawing the laser or punch actually runs from, and give its width and depth as dimensions rather than leaving them to the shop. State the material thickness and the inside bend radius for every bend, since both rules above are derived from them and neither can be assumed from the sheet gauge. Note the bend direction and, where crack risk is high, ask for bends across the grain rather than along it. Keep the bend radius consistent across the part so a single tool set can form it, and flag any flange that falls below the four-thickness minimum early, because that is a tooling decision rather than a drawing one. Finally, mention any surface finish that follows, since a powder coat or paint film will be thinner or missing on the inside of a narrow notch and the gap will be more visible after coating than before it.
See sheet metal fabrication for the laser cutting and forming route we run, metal bending for press brake work quoted from your flat pattern, and metal stamping for tooled parts where a tear relief or a punched notch is built into the die.
Scope and sources. The rule that a relief width of at least 1 x material thickness and a depth of at least the bend radius plus the thickness prevent tearing, the worked example of a 2 mm part with a 2 mm radius needing a relief 2 mm wide and 4 mm deep, the three relief types with their trade-offs, and the bulge that makes a lid rock on the corner are set out in a corner relief design guide. The bend relief rules of width at least 1T and depth at least the bend radius plus 1T, the minimum flange length of about 4T plus the radius, the feature-to-bend distance of 2.5T plus the radius and the minimum inside bend radii of 1T for soft alloys and 1.5T to 2T for hard tempers come from a sheet metal design for manufacturability guide, with the same relief and minimum radius rules stated independently in a note on sheet metal bending technique. The relief width and depth rules expressed against material thickness, the recommended values of twice the thickness and the radius plus 1.2 times the thickness, and the advice to work from the bend line itself come from a sheet metal design practice guide. These are planning rules for standard tooling; the relief that a specific die and material need should be confirmed by the fabricator on your flat pattern.