A bracket can pass every strength check and still be impossible to make. The flange is too short to sit on the die, a hole stretches into an oval because it is too close to the bend, or the last flange cannot be formed because the part hits the punch. These problems are found at the press brake, usually after the laser has already cut the blanks.
This article covers the folding rules that matter most when designing brackets and small folded parts. The numbers given are rules of thumb for mild steel in air bending. Your fabricator's tooling list and bend data always take priority, so check with them before you release drawings.
Flange length and the V-die
In air bending, the sheet is supported on the two shoulders of a V-die while the punch pushes it down between them. The die opening V controls almost everything: the inside radius, the force needed, and the shortest flange that can be formed. A common rule of thumb for mild steel is a die opening of about 6 to 8 times the sheet thickness, with wider dies often used for thicker plate.
The minimum flange length follows from the geometry. At 90°, each leg sits at 45° in the die, so the distance from the outside corner to the shoulder is half the die opening divided by cos 45°:
V ≈ 6 to 8 × T (rule of thumb, mild steel)
b min ≈ (V ÷ 2) ÷ cos 45° ≈ 0.71 × V ≈ 0.7 × V
Ri ≈ 0.15 to 0.17 × V (air bending, mild steel)b min is measured to the outside of the bend. In practice add a small margin so the flange does not sit right on the shoulder edge.
| Thickness T | Typical V-die (≈ 8 × T) | Inside radius (≈ 0.16 × V) | Min. flange (≈ 0.7 × V) |
|---|---|---|---|
| 1.0 mm | 8 mm | 1.3 mm | 5.6 mm |
| 1.5 mm | 12 mm | 1.9 mm | 8.4 mm |
| 2.0 mm | 16 mm | 2.6 mm | 11.2 mm |
| 3.0 mm | 24 mm | 3.8 mm | 16.8 mm |
| 4.0 mm | 32 mm | 5.1 mm | 22.4 mm |
| 5.0 mm | 40 mm | 6.4 mm | 28.0 mm |
If a flange has to be shorter than this, there are options: a narrower die (at the cost of a tighter radius and higher force), a longer flange that is trimmed after bending, or a change of detail. It is far cheaper to decide this at the design stage than on the shop floor.
Holes, slots and bend relief
Material near a bend is stretched and drawn towards the bend. A hole or slot too close to the bend line distorts into an oval, and an edge of the hole may pull into the radius. A widely used rule of thumb is to keep the edge of any hole at least 2.5 × T clear of the bend tangent line. A second check is to keep features whose shape matters outside the die shoulders, roughly V ÷ 2 either side of the bend line, because the sheet is deforming over that whole width.
For 2 mm steel on a 16 mm die, 2.5 × T is 5 mm from the tangent line, which puts the hole edge a little over 7 mm from the bend line. The die check gives 8 mm. Use the larger value, or ask your fabricator what their tooling achieves.
Where a bend stops short of the edge of the blank, the material at the end of the bend line has nowhere to go and tears or bulges. A bend relief, a small slot or notch at each end of the bend, prevents this. As a rule of thumb, make the relief at least T wide and run it at least T past the tangent line. Many shops prefer a minimum width of about 1 mm so the laser can cut it cleanly, and a round-ended slot is kinder in fatigue than a sharp square notch.
Bend sequence and tool collisions
Every bend has to be made with the part located against the back gauge, and every flange already formed has to clear the punch, the die and the machine as the part rotates. The order of bending is therefore part of the design, even if it never appears on the drawing.
- U-channels and return flanges: if a flange is taller than the base is wide, the last bend will often clash with a straight punch. Gooseneck punches help, but each has its own clearance profile.
- Box shapes: the final flanges must fit around the punch, so very deep boxes may need segmented tooling or a different joint.
- Flange height: very tall flanges may hit the ram or the top of the machine when the part is turned over for the next bend.
- Locating: each bend needs a straight edge or flange to sit against the back gauge. Notches and angled edges can make this difficult.
Z-bends have a specific limit. After the first bend, the second bend is made with the first flange pointing at the die. If the offset J is less than roughly the minimum flange length for the die plus the thickness, the part will not sit on the shoulders. Smaller offsets need a dedicated offset (joggle) tool, which the fabricator may or may not have. Ask before you design one in.
Keep the inside radius consistent
In air bending the inside radius comes from the die, not from the CAD model. If one part has bends at three different radii in the same thickness, it may need three die set-ups, or the shop will form them all on one die and the flat pattern will be wrong. Use one inside radius per thickness throughout a part, and ideally across a product range, and choose it to match the die the fabricator will use. It simplifies set-up, makes flat patterns predictable and keeps the bend table short.
Grain direction
Rolled sheet has a grain along the rolling direction. Bending across the grain, with the bend line perpendicular to the rolling direction, is less prone to cracking on the outside of the bend than bending along it. This matters most for tight radii, high-strength steels and harder tempers of aluminium. Where it matters, show the rolling direction on the flat pattern and allow for it in nesting, accepting that it may cost some material yield.
Tolerances add up
Each bend carries a tolerance on its position and its angle. Typical press-brake work might hold flange lengths to a few tenths of a millimetre and angles to about ±1°, but this depends on the machine, the material batch and the operator. Two effects are easy to overlook:
- Chained dimensions: a feature dimensioned across three bends, each held to ±0.3 mm, could be out by ±0.9 mm in the worst case, or about ±0.5 mm statistically (√3 × 0.3 ≈ 0.52 mm).
- Angle at a distance: a 1° angle error on a 100 mm flange moves its tip by 100 × tan 1° ≈ 1.75 mm.
Dimension critical features from a single datum rather than chaining them across bends, keep mating holes on the same flange where possible, and use slotted holes or locating tabs where tolerances would otherwise stack up. Only put tight tolerances on the dimensions that genuinely need them.
Checklist before release
- Every flange is longer than the minimum for the die that will form it.
- Holes and slots are clear of the bend zone, or are cut after bending.
- Partial bends have reliefs of adequate width and depth.
- A feasible bend sequence exists, and return flanges and Z-bends clear the available tooling.
- One inside radius per thickness, matched to the fabricator's dies.
- Grain direction is shown where cracking is a risk.
- Critical dimensions are taken from a datum, not chained across bends.
If you would like a second pair of eyes on a bracket before it goes to the press brake, send us your drawings.