The minimum bend radius is a material-and-process limit, not simply the smallest punch available. A useful recommendation identifies the alloy, temper, thickness, direction and forming conditions. Start with that information before calculating the flat pattern.
5052 aluminum: a qualified reference example
The following selected values come from the Atlas Steels 5052 datasheet, revised 24 June 2021, page 3. Its bending-radii note specifies bending at 90° to the rolling direction. This describes orientation to the grain; do not confuse it with the finished included angle. Atlas presents these as recommendations, not guaranteed process limits.
| Alloy and temper | Sheet thickness t | Source ratio R/t | Calculated inside radius R |
|---|---|---|---|
| 5052-H32 | 1.6 mm | 1.0 | 1.6 mm |
| 5052-H34 | 1.6 mm | 1.5 | 2.4 mm |
| 5052-H32 | 3.2 mm | 1.5 | 4.8 mm |
| 5052-H34 | 3.2 mm | 2.0 | 6.4 mm |
These four entries are not a chart for all sheet metal. Do not interpolate an unlisted thickness, substitute a different temper, or transfer the values to a bend along the rolling direction without supplier confirmation. Equipment, tooling and edge condition still affect the result.
Turn the reference into a design decision
Consider an illustrative 3.2 mm 5052-H32 bracket with a proposed 3 mm inside radius. The proposed ratio is 3/3.2 = 0.938t, below the selected 1.5t reference. Flag the design for review rather than assuming a small punch will make it acceptable. A 4.8 mm radius matches the reference arithmetic, but remains a candidate for the actual drawing angle and manufacturing setup, not an approved production value.
If a mating component demands the tighter corner, the decision is about the design and process: can the mating part change, can a larger radius fit, or is a different material condition permitted? A substitution needs engineering approval; it is not a K-factor adjustment.
Check material limits separately from achieved radius
In air bending, the formed radius is influenced by the die opening and material response. WILA explains why the natural product radius differs from the punch-tip radius. Thus a material recommendation and a tooling prediction answer different questions. Check both, then update the bend allowance calculation using the achieved radius and an appropriate process factor.
| Before releasing the drawing | Record or verify |
|---|---|
| Stock identity | Alloy, temper, certificate, actual thickness and rolling direction |
| Geometry | Inside radius, finished angle, flange lengths, holes and bend-end relief |
| Process | Air bending or another method; punch, die and available load ratings |
| Trial result | Achieved radius/angle, edge cracking, surface damage and dimensional repeatability |
A test-bend record that can be reused
Use a representative coupon with the production material orientation and edge preparation. Record the drawing revision and tool IDs, measure the relaxed part, and inspect the tensile surface and bend ends against agreed acceptance criteria. Keep the actual measurements rather than only a pass/fail label. This page supplies a record structure, not claimed shop test data.
For the related design checks, see back-calculating K-factor, bend-relief geometry and the V-die selection guide. Confirm critical applications through the material supplier, fabricator and responsible engineer; see our engineering disclaimer.
Content updated October 8, 2026. Sources and numerical examples are explained above; examples are not production test results. Editorial method · Report a correction.