Guide
What bend relief width and depth stop formed parts tearing at the corner?
A bend relief is a small notch, slot or hole cut into the flat blank where a bend line runs into an edge or meets another bend, so the metal in the bend can stretch and compress without dragging on the unbent metal next to it. Without one, that corner metal has nowhere to go and it tears, bulges or cracks; with one that is too narrow or too shallow, the tear simply starts at the end of the relief instead.
By Saola Manufacturing engineering team · Published · Updated
This guide is for design engineers, quality engineers and buyers looking at a bracket, chassis, cover or clip with a ragged tear where a flange ends, or a crack in the corner where two flanges meet. It explains how to tell a relief problem from a bend radius problem, ranks the usual causes, shows how to check the part against its flat pattern, gives starting sizes for relief width and depth, and ends with the notes that belong on the drawing and the RFQ. The sizes here are published government guidance and typical industry starting points, not the capability of any particular press shop.
On this page
What does a missing or undersized bend relief look like on a formed part?
A relief problem shows up as a tear, a bulge or a crack that starts exactly where a bend line ends: at the edge of the blank beside a flange, or in the corner where two flanges meet. If the crack instead runs along the middle of the outside of the bend, the bend radius or the material is the more likely culprit.
When sheet is bent, the material inside the bend zone is stretched on the outside and compressed on the inside, and it thins slightly. The flat material right next to the end of the bend is not being bent at all. Along the line where the two meet, the bending metal pulls on the flat metal, and unless something separates them, the weaker of the two gives way. The FAA’s airframe handbook describes relief holes as the material removed at intersecting bends to make room for the metal in the flanges, and says they relieve stresses as the metal is bent and prevent it from tearing (FAA-H-8083-31A, chapter 4).
There are three common signatures. A flange that ends partway along an edge tears along the line where the flange stops, often with a lip of the neighboring flat material dragged upward. A box or tray corner where two flanges meet shows a crack running diagonally out of the corner, or a pucker of compressed metal where the two bend zones overlap. A relief that is present but too short leaves a short tear running on from the end of the slot into the base, because the slot stopped inside the bend zone. All three are geometry problems in the flat pattern, and none of them is fixed by a softer press setting.
Not every corner defect is a tear. Look for a raised burr at the root of the relief, a wavy or bulged edge on the base next to a flange, and coating that has cracked only at the corner after finishing. Those are early signs of the same overlap and can turn into cracks under vibration in service.
What causes formed parts to tear where the bend meets the edge, from most to least common?
In rough order of frequency, corner tears come from no relief on the flat pattern, a relief that ends inside the bend zone, a relief that is too narrow or square-ended, a bend radius or temper that is already at its limit, and a burr or rough edge at the root of the relief. Most of these are decided on the drawing, before any die is built.
- No relief at all. The 3D model folds cleanly because the software tears the corner silently, then the flat pattern goes out without a relief, or the relief is lost when the flat is redrawn for the die. The FAA advisory circular on repair practice tells mechanics to drill relief holes at the ends of bend lines and at corners before bending, to prevent cracks from starting (FAA AC 43.13-1B, paragraph 4-55).
- Relief too shallow. The slot has to run all the way through the bend zone and end beyond the bend tangent line on the base side. A relief sized for one radius becomes too short when the radius is later opened, for example to stop cracking on a hard temper, because the bend zone and the setback both grow with the radius.
- Relief too narrow or with a sharp root. A hairline slot lets the two sides rub and pinch during forming, and a slot that ends in a sharp square root concentrates the forming strain at that corner, so the tear tends to begin there. A narrow slot is also hard to pierce, so the die designer may quietly change it.
- Radius, temper or grain already at the limit. A relief removes the corner conflict, but it cannot rescue a bend that would crack anyway. If the bend runs parallel to the rolling direction in a hard temper, the corner is simply where the crack shows first.
- Burr or rough edge at the root. A punched or sheared relief has a burr side and a fractured band. If the burr ends up on the outside of the bend at the root of the relief, it acts as a ready-made crack starter; the shipped guide on burr direction on a stamping drawing covers how to control it.
One more cause sits outside the part: a relief hole or slot that is mispositioned relative to the flange edge, leaving a thin sliver of material between the slot and the flange. That sliver bends with the flange but is held by the base, and it tears exactly like a part with no relief.
How do you diagnose a corner tear from the part and the flat pattern?
Mark where the tear starts, measure the actual inside radius and the relief on a formed part, and compare both with the flat pattern the supplier actually used. In most cases that comparison shows whether the relief was missing, too short, too narrow or in the wrong place without any lab work.
Start with the part. Sketch the corner and mark the crack origin: at the end of the relief slot, at the blank edge where a flange stops, or diagonally out of a box corner. Measure the inside bend radius with radius gauges or an optical comparator, because the punch nose on the press may not match the drawing. Then measure the relief depth on the formed part from the outside face of the flange, and its width. Note which face carries the burr at the root of the relief.
Next, get the flat pattern. Ask the supplier for the DXF or blank drawing that the die was built to, not the one you sent, and overlay it on yours. Differences in relief size, position or shape are common because a relief that suited laser-cut prototypes is often redrawn for a punch. Finally, check the setback. For a 90-degree bend, the FAA handbook gives the setback, the distance from the outside mold line back to the bend tangent line, as the inside radius plus the thickness, R + T (FAA-H-8083-31A). A relief whose depth, measured from the outside face of the flange, is less than R + T stops inside the bend zone, which is exactly the geometry that produces a tear running on from the end of the slot.
| What you see | Most likely cause | How to confirm | First fix |
|---|---|---|---|
| Tear along the line where a flange stops, neighbor metal dragged up | No relief on the flat pattern | Supplier's blank or DXF has no slot at the bend-line end | Add a relief slot at the end of the bend line |
| Short tear running on from the end of an existing slot | Relief ends inside the bend zone | Relief depth from outside face of flange is less than R + T | Lengthen the relief past the bend tangent line |
| Crack starting at a square corner at the root of the slot | Sharp-cornered relief end | Crack origin is the slot corner, not the edge of the bend | Use an obround or round-ended relief, or end the slot in a hole |
| Edges of a narrow slot rubbed, pinched or bulged | Relief too narrow | Slot width well under one thickness; witness marks on both sides | Widen the relief to about one thickness |
| Diagonal crack or pucker in a box corner where two flanges meet | No corner relief, or hole not reaching the tangent-line intersection | Bend zones of the two flanges overlap on the flat pattern | Add a corner relief hole located from the intersection of the inside bend tangent lines, with its position dimensioned on the flat pattern |
| Cracks at corners and along the middle of the bend on the same part | Radius too tight for the temper or grain direction | Temper on the mill certificate, and measured radius below the minimum recommended for that alloy and temper (for aluminum, AC 43.13-1B table 4-6) | Treat as a bend radius problem first, then recheck relief depth |
What bend relief width and depth should you use?
As typical industry guidance, make a bend relief slot at least one material thickness wide and long enough to end beyond the bend tangent line on the base, which for a 90-degree bend means a depth of at least the inside radius plus the thickness (R + T) from the outside face of the flange, plus a small clearance. For a corner where two flanges meet, use a relief hole whose edge touches, and slightly passes, the intersection of the inside bend tangent lines.
Depth is the dimension that fails most often, and it is the easiest to get right from geometry. The relief has to free the whole bend zone, so it must reach the tangent line where the base stops curving. For a 90-degree bend that line sits one setback, R + T, in from the outside face of the flange, so the relief must be at least that deep, and it must be lengthened whenever the radius grows. Typical CAD and fabrication guidance adds a small clearance beyond R + T to absorb bend-line tolerance.
For corner relief holes the FAA handbook gives concrete layout rules written for aluminum alloy sheet. It states that relief holes must touch the intersection of the inside bend tangent lines and, to allow for error in bending, should extend 1/32 to 1/16 inch behind those lines, and calls it good practice to use the intersection as the center of the hole (FAA-H-8083-31A, relief hole location). It also says the larger and smoother the relief hole, the less likely a crack is to form in the corner. On size, the handbook ties the hole to the bend radius, and its layout figure (FAA-H-8083-31A, figure 4-146) shows a 5/8 inch hole for a 5/16 inch bend radius, which matches its statement elsewhere that the diameter is approximately twice the bend radius. Read the handbook with care on two points: its layout method places the hole so that its edge, not its center, touches the intersection, by moving the center outward along the bisector by one hole radius (FAA-H-8083-31A, layout method); and the same section also says the most common method is to use the bend radius for the hole dimension, with a 1/8 inch minimum. Because the source allows both readings, dimension the hole diameter and its position from the tangent-line intersection on your own flat pattern rather than leaving it to a rule of thumb.
Width is a trade-off between forming and tooling. A slot narrower than the sheet is thick can be laser cut, and typical fabrication guidance for thin laser-cut parts accepts widths down to about half the thickness. In a stamping die, though, a slot is pierced or notched by a punch, and a punch much narrower than the sheet is thick is fragile; typical die design guidance therefore keeps punched reliefs at or above one thickness, the same reasoning that sets minimum punched hole size in the hole-to-bend distance guide.
| Feature | Starting value | Basis |
|---|---|---|
| Relief slot width | At least 1 T for punched reliefs; about 0.5 T acceptable for laser-cut thin sheet | Typical industry guidance; punch strength sets the lower limit in a die |
| Relief slot depth, 90-degree bend | At least R + T from the outside face of the flange, plus a small clearance | Setback = R + T to the bend tangent line (FAA) |
| Relief end shape | Full round (obround) or ended in a hole; avoid sharp inside corners | Typical industry guidance; FAA notes larger, smoother holes crack less |
| Corner relief hole position | Touching the intersection of the inside bend tangent lines and extending 1/32 to 1/16 in behind them; the handbook gives both a centered layout and an edge-touching layout, so dimension the position | FAA-H-8083-31A, relief hole location |
| Corner relief hole diameter, aluminum up to 0.064 in thick | Not less than 1/8 in; commonly based on the bend radius | FAA-H-8083-31A |
| Corner relief hole diameter, aluminum 0.072 to 0.128 in thick | Not less than 3/16 in (printed as “3/160-inch” in the 2018 handbook, evidently a typographical error) | FAA-H-8083-31A |
When a relief is not the best fix. Sometimes the cleaner answer is to remove the conflict. Running the flange the full length of the edge, or setting the end of the flange back from the edge by a full relief depth, removes the need for a slot. Some CAD packages also offer a “rip” or “tear” option that models the corner as a cut with no material removed. No real cutting process has zero kerf, so that geometry has to be reinterpreted by whoever programs the blank; replace it with a dimensioned slot before the flat pattern is released, particularly for hard tempers, visible corners or parts that see vibration.
Worked example. A bracket in 1.5 mm sheet with a 1.5 mm inside radius and a 90-degree flange that stops partway along the edge has a setback of R + T = 3.0 mm by the FAA 90-degree setback rule (FAA-H-8083-31A). Following that rule and typical industry guidance, a relief slot for that bend needs to be at least 3.0 mm deep from the outside face of the flange, plus a small clearance for bend-line position, and, if it will be punched, at least about 1.5 mm wide with a round end. If a later revision opens the radius to 3.0 mm to stop cracking in a harder temper, the same setback rule (FAA-H-8083-31A) gives 4.5 mm and the same slot is now 1.5 mm too short: the classic case of a tear appearing after a change that was meant to cure cracking.
What should the drawing and RFQ say so corners do not tear?
Show every relief on the flat pattern with its width, depth from a stated face, and end shape, state the inside bend radius and the material temper it was sized for, and say whether the supplier may change the relief to suit the die. A drawing that only shows the folded part leaves relief design to whoever builds the tool.
- Relief geometry. Dimension width, depth and end radius on the flat pattern, or give a general note such as “bend reliefs: width 1T min, depth to clear bend tangent line, full round end, unless otherwise shown”.
- Reference face. Say whether relief depth is measured from the outside face of the flange, the inside face or the tangent line. Those differ by R or by T, and the difference is often the whole clearance.
- Radius and temper together. Put the inside radius and the material temper on the same drawing revision as the relief, and add a note that any radius change requires the relief depth to be rechecked.
- Corner reliefs. For boxes and trays, show the corner relief hole or notch and its position relative to the intersection of the inside bend tangent lines.
- Burr side. State “burr side to inside of bends” or mark it on the view, so the root of each relief is not on the tension side.
- Acceptance. Add “no tears or cracks at bend-line ends or corners when examined at low magnification”, with the magnification stated, so the plant and receiving inspection apply the same criterion.
On the RFQ, say whether the corners are cosmetic, which finish follows forming, and whether you will accept a relief change, a larger radius or a flange set back from the edge if the supplier proposes it. Ask for any proposed change to be shown on the supplier’s flat pattern and approved in writing before the die is cut, because after that the relief is built into the steel.
If tears are found on parts already made, separate the two decisions. For the lot on hand, agree a sort criterion (every bend-line end and corner examined at a stated magnification) and decide disposition of torn parts with the design owner; a tear sits in the most strained part of the bend and is not a cosmetic defect. For future lots, correct the flat pattern first, then confirm the change on first-off parts formed with the revised notch or relief punch before the run is released.
How are bend relief and corner tearing questions handled on a Saola order?
On a Saola order, stamped and formed parts are made at partner stamping plants we manage, and the quote names the production site and the country of origin. The relief, radius and temper notes on your drawing are what the forming plant works to, so a dimensioned flat pattern is the most direct way to keep corner tears off the receiving dock.
Blanking, piercing, notching and forming run at partner plants, as described on the stamping page; those plants are not named and are not necessarily in Vietnam, which is why each quote states where the work is done. Machined features on the same assembly are cut at our lead CNC plant, T.K Viet Nam Precision Company Limited, in operation since 2017, and finishes are applied by partner finishing plants we manage. The quote comes back with a short manufacturability note, and that is where a comment on a relief that looks too shallow for the radius, or too narrow to punch, will appear. If you are open to a different relief shape or a flange set back from the edge, say so on the RFQ.
If a delivered lot tears at the corners, send photos of the crack origin, the lot identity and the drawing revision. We take it up with the plant that formed the parts and work through the diagnosis table above, starting with the flat pattern the die was built to, the measured radius and the burr side. ISO 9001 certification is in progress, not held. Send the drawing with its flat pattern through the quote form.
Frequently asked
What is the difference between a bend relief and a corner relief?
A bend relief frees the end of a single bend where it runs into an edge or into unbent material. A corner relief frees the spot where two bends meet, as in a box corner, and is usually a hole or notch at the intersection of the inside bend tangent lines.
Is bend relief depth measured from the bend line or from the edge?
Conventions differ between CAD tools and shops, which is why the drawing should name the reference face. Whatever the reference, the relief must end beyond the bend tangent line on the base; for a 90-degree bend that is R + T in from the outside face of the flange.
Do thin parts need bend reliefs?
Thin, soft sheet often forms a small flange without one, because the corner metal can deform instead of tearing. It still leaves a bulge or ragged corner, so a relief is worth adding wherever the corner is visible, the temper is hard or the part sees vibration.
Why did my laser-cut prototypes form fine but the stamped parts tear?
A narrow relief that a laser cuts easily may be widened, shortened or reshaped when it is redrawn for a punch, and a production die may use a different radius from the prototype brake. Compare the die flat pattern with the prototype one before blaming the material.
Can a torn corner be repaired?
A tear is a crack in the most strained part of the bend, so welding or filling it is a disposition decision for the design owner, not a routine fix. The reliable answer is to correct the flat pattern so the next lot forms without tearing.
Sources
- Aviation Maintenance Technician Handbook — Airframe, Volume 1 (FAA-H-8083-31A), Chapter 4: folding a box, relief hole location and layout, setback, Federal Aviation Administration, 2018
- Advisory Circular AC 43.13-1B, Acceptable Methods, Techniques, and Practices: Aircraft Inspection and Repair, paragraphs 4-55 (bending metal, table 4-6) and 4-56 (setback), Federal Aviation Administration, 1998 (Change 1, 2001)