The quick answer
Use the minimum bend radius chart below as the absolute floor, not a target. The values assume room-temperature bending with standard press-brake tooling, material perpendicular to the grain, and a clean bend without external features nearby. For production-safe designs, bump the radius up by 50% — that gives you margin against tolerance stack-up in sheet thickness and lot-to-lot variation in material ductility.
Every value here is an inside radius (the concave side of the bend), which is how our press-brake operators and tooling library reference radii. If your drawing specifies outside radius or centerline radius, note that explicitly — misreading the callout is the most common cause of mis-bent parts.
Minimum bend radius by material — room temperature
| Alloy / Temper | Min R (inside) | Typical use |
|---|---|---|
| 5052-H32 | 0.5 × t | Enclosures, brackets, bendable panels |
| 5052-O (annealed) | 0 × t (flat) | Hemming, tight folds |
| 6061-T4 | 1.0 × t | Bend then age-harden to T6 |
| 6061-T6 | 2.0 × t | Structural — but bends carefully |
| 6063-T5 | 1.5 × t | Anodized trim, architectural |
| 7075-T6 | 4.0 × t | Aerospace — bend with caution |
| 3003-H14 | 0.5 × t | Tank walls, deep-draw formed parts |
| Alloy | Min R (inside) | Notes |
|---|---|---|
| CRS (cold-rolled steel, 1008–1018) | 0.5 × t | Workhorse — bends easily |
| HRS (hot-rolled steel) | 1.0 × t | Mill scale; de-scale before bending if possible |
| Galvanized (G90) | 1.0 × t | Zinc coating cracks at tight radius |
| HSLA 50 ksi | 1.0 × t | Automotive structural |
| DP590 dual-phase | 1.5 × t | Crash structures |
| DP780 dual-phase | 3.0 × t | B-pillar, reinforcements |
| DP1180 dual-phase | 5.0 × t | Press-hardened grades need hot forming |
| Alloy | Min R (inside) | Notes |
|---|---|---|
| 304 / 304L stainless | 0.5 × t | Work-hardens; avoid re-bending |
| 316 / 316L stainless | 0.5 × t | Same as 304 in bendability |
| 430 ferritic stainless | 1.0 × t | Less ductile than austenitic |
| Copper C110 soft | 0 × t (flat) | Bends to full contact |
| Brass C260 | 0.5 × t | Decorative bent parts |
| Titanium Grade 2 | 2.5 × t | Bend hot for tight radii |
Why minimum bend radius matters
The outside surface of a bend has to stretch. How much it stretches depends on the ratio of radius to thickness: tighter radius means more stretch. When stretch exceeds the material's elongation-to-failure, the outer surface cracks. Cracks can be microscopic (visible under magnification but passing visual inspection) or macroscopic (rejected immediately), but both indicate local damage that reduces fatigue life by 10–100×. A part with marginal cracking may survive static testing and fail in service under vibration.
The inside of the bend compresses, which rarely causes problems except with very brittle materials or in sharp re-entrant geometries. Compression wrinkles occasionally appear on thin, highly-ductile sheets bent past their optimum radius — a separate failure mode from outside cracking.
K-factor and bend allowance — why your flat pattern matters
A bent part is longer across the bend than a straight piece of material would suggest. The neutral axis — the internal plane that neither stretches nor compresses — sits somewhere between the inside and outside of the bend, usually 33–44% of thickness from the inside surface. The ratio is called the K-factor, and it determines how much material the bend consumes.
Practical values we use: K = 0.42 for soft aluminum (5052), 0.40 for 6061-T6, 0.38 for CRS and stainless, 0.33 for hardened steel and 7075. Tight radii push K toward 0.33 because the neutral axis shifts inward; generous radii push K toward 0.50. Our CAD unfolder takes the bend radius as input and adjusts K-factor accordingly. If you supply your own flat pattern, agree on K-factor with us in advance — a 0.05 error gives ~0.3mm deviation per bend on 3mm stock, and with four bends in series the part can be 1.2mm off at the end.
Bend-to-feature clearance
Holes and slots placed too close to a bend line will distort when the bend forms. The minimum clearance from the bend line to the edge of any feature is typically 2.5 × material thickness + bend radius. For 3mm stock bent on a 3mm radius, that's 10.5mm clearance to the center of any hole. Inside this envelope, holes deform into ovals, slots curve, and tapped threads become difficult to engage.
If your design needs features closer to the bend, two options: (1) drill or tap the holes after bending in a secondary operation — adds 30–50% to part cost but preserves hole accuracy; (2) use a relief slot at each end of the bend to isolate the feature from bend-induced distortion. We flag clearance violations on DFM review and propose one of these fixes.
Press-brake tooling — the practical minimum
Theoretical minimum bend radius (from the chart) and practical minimum (what our tooling can actually do) are different numbers. Press-brake punches have a tip radius — typically 0.8mm, 1.5mm, 3mm, or 6mm — and the bent part inherits approximately that radius plus a correction for springback. If the theoretical minimum is 1.0mm but our smallest punch tip is 1.5mm, you get 1.5mm radius regardless.
For prototypes, we match the closest available tooling and note the actual radius on the inspection report. For production runs, we can spec custom tooling if the part geometry justifies it. The tooling library changes occasionally — confirm exact tip radius availability during the quote.
Springback — the reason your bend angle isn't quite 90°
Sheet metal doesn't stay at the exact angle the press brake bends it to. Elastic strain in the material partially recovers when the punch releases, causing the part to open up by typically 1–3°. The amount depends on material, thickness, radius, and temper: harder materials and tighter radii spring back more. A target 90° bend is achieved by overbending to approximately 87° on CRS or 88° on 5052.
Modern press brakes compensate automatically using material databases, but the first-piece inspection step verifies actual angle and adjusts bend-angle commands for the run. Drawings should specify the final part angle (usually with ±0.5° tolerance on 90° bends); we handle the overbend offset on the shop floor.