The rule of thumb is simple: make the inside bend radius equal to the material thickness. A 2 mm steel bracket gets a 2 mm inside radius, a 1.5 mm aluminium cover gets 1.5 mm. It works surprisingly often, and it's still the default I set in Fusion 360 when I start a new sheet metal part. It also fails in a few predictable places: hard aluminium tempers, thick plate, short flanges and holes close to the bend. Those are the ones worth walking through, because they're exactly where a part that unfolded perfectly in CAD comes back from the shop with a phone call.
Why one times thickness works at all
When you bend a sheet, the outside surface stretches and the inside compresses. The tighter the radius relative to thickness, the harder the outer fibres are stretched. Stretch them past what the alloy can take and they crack. At 1T, common mild steels, 304 stainless and the softer aluminium grades bend without cracking, which is the first reason the rule exists.
The second reason is the one designers tend to miss.
On a press brake you don't choose the radius by drawing it. In air bending, which is how most shops form most parts, the inside radius is set by the V-die opening, roughly 15 to 17% of the opening for mild steel. Shops typically pick a V opening of 6 to 8 times thickness, so for 2 mm steel on a 16 mm die you get an inside radius of about 2.5 mm whatever your model says. 1T is simply close to what the tooling produces anyway, and that's why the rule has survived for so long.
Where it fails: 6061-T6 and other hard tempers
6061-T6 aluminium is the classic trap. It machines beautifully, every stockist has it, and it cracks on the outside of a 1T bend. For 6061-T6 I'd start at 2.5 to 3 times thickness on thin sheet, go higher above 3 mm, and still ask the shop. The better answer is usually a different alloy: 5052-H32 bends happily at 1T and is what most sheet metal shops keep in stock for formed parts anyway.
A couple of years ago I reviewed a small electronics enclosure drawn in 3 mm 6061-T6 with a 1 mm inside radius on every bend. In CAD it flattened without a single warning. The first samples came back with a rough, orange-peel surface along the outside of each bend and two hairline cracks, and switching to 5052-H32 with a 3 mm radius fixed it on the next batch without changing anything that mattered functionally. Stainless is less dramatic. 304 at 1T forms fine, but it springs back more than mild steel, so it needs more overbend, and on tight-tolerance flanges you'll see the angle drift between batches.
Where it fails: thick plate
Above about 6 mm, 1T stops being a safe default. Thick plate goes on bigger dies with wider openings (often 8 to 10 times thickness), so the natural radius grows, and high-strength structural grades want 1.5 to 2T or more. Grain direction starts to matter too. Bend across the rolling direction where you can, because bending parallel to it on a tight radius is how you get cracks on a part that passed every other check.
Draw 10 mm plate with a 10 mm inside radius and a decent shop will either quote the radius they can actually make or email you a question.
Either way, you've lost a day.
Thick plate also tightens the hole rule. Laser-cut holes in 8 mm plate close to a bend don't just go oval, they can drag the bend line itself off straight, so I either keep them well clear or have them drilled after forming. Drilling afterwards costs an extra setup, but on a batch of fifty brackets it's usually still cheaper than scrapping the first five.
Where it fails: flanges and holes near the bend
The radius rule says nothing about the geometry around the bend, and most of the rejected sheet metal parts I see fail here rather than on the radius itself. It's the bulk of what a DFM review on a bent part actually catches.
Minimum flange length depends on the die. The flange has to span the V opening while it's being formed, so a rough minimum is half the opening plus a bit: for 2 mm steel on a 16 mm die, keep flanges at least 9 to 10 mm, measured to the outside. Shorter than that and the shop needs a narrower die, which tightens the radius, which brings you straight back to cracking.
Holes near a bend distort. Keep the edge of any hole at least 2.5 times thickness plus the bend radius from the bend line. Why so much? On 2 mm steel with a 2 mm radius that's 7 mm. Closer, and round holes go oval.
Add bend reliefs where a bend runs out at an edge.
Relief width at least equal to thickness, depth at least thickness plus radius. Without them the material tears at the corner, and the tear tends to show up after powder coating, when it's most expensive to find.
A quick reference I actually use
| Material | Starting inside radius | Notes |
|---|---|---|
| Mild steel (DC01, S235) up to 6 mm | 1T | Default; the V-die sets it anyway |
| Stainless 304 | 1T | More springback, allow angle tolerance |
| Aluminium 5052-H32 | 1T | The forming alloy, use it if you can |
| Aluminium 6061-T6 | 2.5T to 4T | Cracks at 1T; ask the shop or change alloy |
| Plate over 6 mm, high-strength grades | 1.5T to 2T or more | Check grain direction and die availability |
Treat those as starting points, not specs. The shop's tooling list beats any table on the internet, mine included. One counter-intuitive point: going much bigger than you need isn't free either. Large radii spring back more, so a 90° bend at 5T in stainless can come off the brake at 93° unless the operator compensates. Bigger is safer for cracking and worse for angle accuracy.
What I'd actually do on a new part
Ask the shop for their V-die list and the inside radius they get for your material and thickness, then set that radius in CAD before you design anything else. In Fusion 360 that means one sheet metal rule per material, with the real radius and a K-factor of around 0.4 to 0.44 for air bending, so the flat pattern matches what the brake produces and hole positions survive forming. It's the first step of every mechanical design job I take on with formed parts. If a shop can't give you a die list (some small job shops won't bother), use 1T for mild steel and 5052, assume a 16 mm V-die for 2 mm material, and mark the radius as a reference dimension so they can adjust.
Don't tolerance the inside radius unless it's functional. A note like "inside radius 2 mm, reference" lets the shop use standard tooling, while ±0.1 mm on a bent radius forces bottoming or a custom die, and you'll pay for both.
One radius per part, if you can manage it.
I check all of this, plus the rest of my sheet metal DFM checklist, before a part goes out for quotes. The general DFM checklist covers the other processes. If you'd like a second pair of eyes on a specific bracket or enclosure, you can request a free initial DFM review of one part.