Reference
Bend radius chart
Minimum inside bend radius by material and temper, expressed as multiples of thickness — plus a worked table in millimeters for the gauges you actually order.
The minimum inside bend radius is the tightest radius a sheet can be formed to on the inside of a bend without cracking the outer surface. It is a property of the material and its temper, not of the press brake, and it is almost always expressed as a multiple of the material thickness — written t. A rule of “1t minimum” means the inside radius should be at least one material thickness. Softer metals bend tighter; harder tempers need a larger radius or they fail.
Minimum inside bend radius by material
Values are minimum inside radius as a multiple of thickness (t) for a 90° air bend, bending across the grain. Bending with the grain needs a larger radius. Treat the low end of each range as the aggressive limit and the high end as the safe design target.
| Material / temper | Min inside radius |
|---|---|
| Low-carbon / mild steel (soft, CRS) | 0.5t – 1.0t |
| Hot-rolled steel (A36) | 1.0t – 1.5t |
| Galvanized steel | 1.0t |
| Stainless 304 / 316 (annealed) | 0.5t – 1.0t |
| Aluminum 3003-H14 | 0.5t – 1.0t |
| Aluminum 5052-H32 | 0.5t – 1.5t |
| Aluminum 6061-O (annealed) | 1.0t |
| Aluminum 6061-T6 (hard temper) | 2.0t – 3.0t |
| Copper / brass (soft) | 0.5t – 1.0t |
Source: multiples of thickness follow common sheet-metal design-for-manufacturing practice (Machinery’s Handbook forming tables; FMA and aluminum-producer bend-radius data). Figures are across-grain minimums for a 90° bend and vary with lot, temper, and grain direction — verify against your material’s certified minimum bend radius before committing a tight callout.
Worked radius for common gauges
The rule only helps once it is a number. Below, the inside radius in millimeters at three common multipliers — 0.5t (soft tempers), 1t (mild-steel default), and 2t (hard tempers) — for the gauges most enclosure and bracket work uses. Thickness is shown as inch / mm using carbon-steel gauge decimals.
| Gauge | Thickness (in / mm) | r at 0.5t (mm) | r at 1t (mm) | r at 2t (mm) |
|---|---|---|---|---|
| 20 ga | 0.036 / 0.91 | 0.46 | 0.91 | 1.82 |
| 18 ga | 0.048 / 1.21 | 0.61 | 1.21 | 2.43 |
| 16 ga | 0.060 / 1.52 | 0.76 | 1.52 | 3.04 |
| 14 ga | 0.075 / 1.90 | 0.95 | 1.90 | 3.79 |
| 12 ga | 0.105 / 2.66 | 1.33 | 2.66 | 5.31 |
| 11 ga | 0.120 / 3.04 | 1.52 | 3.04 | 6.08 |
| 10 ga | 0.135 / 3.42 | 1.71 | 3.42 | 6.83 |
| 3/16 in | 0.188 / 4.76 | 2.38 | 4.76 | 9.53 |
| 1/4 in | 0.250 / 6.35 | 3.18 | 6.35 | 12.70 |
Worked values are thickness × multiplier, using the Manufacturers’ Standard Gauge decimal for carbon steel. Apply the material multiplier from the table above to pick the right column — a 6061-T6 part reads the 2t column, a soft-steel part the 1t or 0.5t column. Verify critical dimensions against your drawing.
How to read the chart
Start with the material table to get your multiplier, then take the millimeter value from the worked table under that multiplier. Example: a 3.0 mm (11 ga) 5052-H32 aluminum bracket sits at roughly 0.5t–1.5t, so a safe inside radius is about 1.5–4.6 mm — design to the larger end unless weight or packaging forces the tight limit. The same gauge in 6061-T6 should read the 2t column (about 6 mm) to avoid cracking.
Common mistakes
- Specifying a sharp (zero) inside radius. Every bend has a radius; a “sharp” callout forces coining, which needs extra tonnage and hard tooling and still is not truly zero. Design to a real radius.
- Using one radius for every material. A radius that is comfortable in 5052 aluminum will crack 6061-T6. Match the radius to the temper.
- Ignoring grain direction on tight bends. If the radius must be tight, orient the bend line across the grain and say so on the print.
- Forgetting bend-radius change shifts every downstream dimension. The inside radius drives the bend deduction, so changing it moves flange lengths and hole positions measured across the bend. Lock the radius early.
Where this fits our shop
Nevatronix Sheet Metal air-bends to the material’s natural radius by default and holds bend angle to ±0.5° and bend position to ±0.1 mm on 50–200 ton CNC press brakes. Pick your stock first with the gauge chart, set the radius here, then send the part for a quote.
Frequently asked questions
- What is the minimum bend radius for sheet metal?
- A safe default minimum inside bend radius for common mild steel is one material thickness (1t). Soft, formable tempers (dead-soft steel, 3003 and 5052 aluminum, annealed stainless) can go tighter, near 0.5t; hard tempers such as 6061-T6 need a larger radius, typically 2t to 3t, or they crack on the outside of the bend. Always state the inside radius, the material, and the temper together — the achievable minimum is a property of the material, not of the press.
- How do I calculate inside bend radius from thickness?
- Multiply the material thickness (t) by the multiplier for your material and temper. For 3 mm mild steel at a 1t minimum, the inside radius is about 3 mm; at 0.5t it is about 1.5 mm. Use the worked table on this page for common gauges, and remember the multiplier is a floor — a larger radius is always easier to form and less prone to cracking.
- Why does bending with the grain need a larger radius?
- Rolled sheet is anisotropic — its grain runs in the rolling direction. A bend line parallel to the grain (bending "with the grain") is more likely to crack on the outer fiber, so it needs a larger inside radius than a bend across the grain. When a tight radius is unavoidable, orient the bend line across the grain, or annode the material. The values on this page are across-grain (transverse) minimums, the more forgiving case.
- What happens if the bend radius is too tight?
- Too tight an inside radius stretches the outer surface past the material’s limit and it cracks, orange-peels, or fractures — most visibly on hard aluminum tempers and work-hardened stainless. It also drives up springback variation and can thin the wall at the bend. If a design needs a radius below the material minimum, the usual fixes are a softer temper, a larger radius, a coined bend on hard tooling, or scoring — all of which we will flag on the quote.
- What inside radius does Nevatronix Sheet Metal form to by default?
- By default we air-bend to the material’s natural radius, which tracks the punch-tip radius — for most gauges that lands near 1t. For tighter inside radii we use hard (bottoming or coining) tooling or a rolling pre-form, and we do not recommend bending below the material’s minimum bend radius without warming or annealing. See our press brake forming page for the full forming capability.
Not sure the radius will form? Ask before you cut.
Send the part and the material grade. If a callout is asking a hard temper to bend tighter than it can, we flag it on the quote — before it becomes a scrapped batch.