SHEET METAL BENDING REFERENCE
Minimum Bend Radius Chart
Every sheet metal designer hits the same question: how tight can I bend this without cracking it? These guidelines answer that question across four variables: material, thickness, temper, and grain direction. Get any one wrong and your parts crack on the press brake. This chart gives you the data for all four variables, plus troubleshooting guidance to fix bends pushing the limit.
✓
Material‑specific bending limits — steel, aluminum, stainless
✓
Thickness × temper × grain direction — all four variables
✓
Troubleshooting guide for bends pushing the limit
Four Key Variables
Material · Thickness · Temper · Grain Direction
Steel
Carbon & galvanized
Aluminum
6061 · 5052 · 3003
Stainless
304 · 316
Temper
Annealed · H-series · T-series
Press Brake Capability
200+ Ton Press Brakes 3–7 day lead time · Free DFM review on every quote
BEND RADIUS CALCULATOR
Interactive Minimum Bend Radius Chart
Select your material, enter your thickness, and choose your grain direction. The lookup returns your minimum inside radius, recommended production radius (minimum + 25% safety margin), V‑die opening, and estimated springback.
1. Select material and temper — Mild Steel CRS (1008/1010), 304/316 Stainless (Annealed), 5052‑H32 / 6061‑T6 Aluminum, C110 Copper (Half‑Hard), or C260 Brass (Half‑Hard).
2. Enter material thickness — in mm or gauge. If you only know the gauge, convert to decimal thickness first; bend radius is always a function of actual thickness, not nominal gauge.
Grain Direction
3. Choose grain direction. Bending across the grain (perpendicular to rolling direction) allows the tightest radius. Bending with the grain requires a 25–50% radius increase because fibers align with tension direction, significantly raising cracking risk.
Read the Results
4. Read the outputs. You’ll see the minimum inside radius (mm & inches), recommended production radius with 25% safety margin, recommended V‑die opening, and estimated springback angle. Use these values to design bend features that are manufacturable on the first try.
Manufacturability Check
5. Check the indicator. Green = comfortably within production capability. Yellow = achievable with care; test bends recommended. Red = at or beyond the material’s forming limit — expect cracking unless adjustments are made.
Reverse lookup mode: Enter your target inside radius and material — the chart tells you the maximum thickness you can use and whether it’s manufacturable with standard tooling. This is especially useful when the bend radius is constrained by mating components and you need to pick a thickness that works.
SHEET METAL BENDING DATA
Minimum Bend Radius Reference Table — Steel, Aluminum & Stainless
Static reference tables covering six common sheet metal materials. Each table provides the minimum inside radius for across‑grain and with‑grain orientation, plus the recommended production radius with a 25% safety margin for reliable manufacturing.
Grain direction: Bending across the grain allows the tightest radius. Bending with the grain requires a 25–50% radius increase. Springback: Stainless steel requires 3–8° overbend compensation. For production reliability, always specify the recommended production radius — not the absolute minimum.
Mild Steel (CRS 1008/1010) — The 1T Standard
| Thickness (mm) | Gauge (approx.) | Min Radius, Across Grain | Min Radius, With Grain | Recommended Production Radius |
|---|---|---|---|---|
| 0.8 | 22 ga | 0.5T (0.4 mm) | 0.75T (0.6 mm) | 1T (0.8 mm) |
| 1.0 | 20 ga | 0.5T (0.5 mm) | 0.75T (0.75 mm) | 1T (1.0 mm) |
| 1.5 | 18 ga | 1T (1.5 mm) | 1.25T (1.9 mm) | 1.5T (2.25 mm) |
| 2.0 | 14 ga | 1T (2.0 mm) | 1.25T (2.5 mm) | 1.5T (3.0 mm) |
| 3.0 | 11 ga | 1T (3.0 mm) | 1.5T (4.5 mm) | 1.5T (4.5 mm) |
| 4.0 | 8 ga | 1T (4.0 mm) | 1.5T (6.0 mm) | 1.5T (6.0 mm) |
Stainless Steel 304 — Higher Springback, Wider Radius
| Thickness (mm) | Gauge (approx.) | Min Radius, Across Grain | Min Radius, With Grain | Recommended Production Radius | Est. Springback |
|---|---|---|---|---|---|
| 0.8 | 22 ga | 1.5T (1.2 mm) | 2T (1.6 mm) | 2T (1.6 mm) | 3–5° |
| 1.0 | 20 ga | 1.5T (1.5 mm) | 2T (2.0 mm) | 2T (2.0 mm) | 3–5° |
| 1.5 | 18 ga | 1.5T (2.25 mm) | 2T (3.0 mm) | 2T (3.0 mm) | 3–5° |
| 2.0 | 14 ga | 1.5T (3.0 mm) | 2.5T (5.0 mm) | 2T (4.0 mm) | 4–6° |
| 3.0 | 11 ga | 1.5T (4.5 mm) | 2.5T (7.5 mm) | 2.5T (7.5 mm) | 5–8° |
| 4.0 | 8 ga | 2T (8.0 mm) | 3T (12.0 mm) | 2.5T (10.0 mm) | 5–8° |
Aluminum 5052-H32 — The Formability Champion
| Thickness (mm) | Gauge (approx.) | Min Radius, Across Grain | Min Radius, With Grain | Recommended Production Radius |
|---|---|---|---|---|
| 0.8 | 22 ga | 0.5T (0.4 mm) | 0.75T (0.6 mm) | 1T (0.8 mm) |
| 1.0 | 20 ga | 0.75T (0.75 mm) | 1T (1.0 mm) | 1T (1.0 mm) |
| 1.5 | 18 ga | 1T (1.5 mm) | 1.25T (1.9 mm) | 1T (1.5 mm) |
| 2.0 | 14 ga | 1T (2.0 mm) | 1.25T (2.5 mm) | 1.5T (3.0 mm) |
| 3.0 | 11 ga | 1T (3.0 mm) | 1.5T (4.5 mm) | 1.5T (4.5 mm) |
| 4.0 | 8 ga | 1.5T (6.0 mm) | 2T (8.0 mm) | 2T (8.0 mm) |
Aluminum 6061-T6 — High Strength, Demanding Formability
| Thickness (mm) | Gauge (approx.) | Min Radius, Across Grain | Min Radius, With Grain | Recommended Production Radius |
|---|---|---|---|---|
| 0.8 | 22 ga | 2T (1.6 mm) | 3T (2.4 mm) | 3T (2.4 mm) |
| 1.0 | 20 ga | 3T (3.0 mm) | 4T (4.0 mm) | 3T (3.0 mm) |
| 1.5 | 18 ga | 3T (4.5 mm) | 4T (6.0 mm) | 4T (6.0 mm) |
| 2.0 | 14 ga | 3T (6.0 mm) | 5T (10.0 mm) | 4T (8.0 mm) |
| 3.0 | 11 ga | 4T (12.0 mm) | 5T (15.0 mm) | 5T (15.0 mm) |
| 4.0 | 8 ga | 4T (16.0 mm) | 6T (24.0 mm) | 5T (20.0 mm) |
Copper C110 & Brass C260 — Highly Formable but Soft
| Material | Thickness (mm) | Min Radius, Across Grain | Min Radius, With Grain | Recommended Production Radius |
|---|---|---|---|---|
| Copper C110 | 0.8–1.5 | 0.5T | 0.75T | 1T |
| Copper C110 | 2.0–3.0 | 0.5T | 1T | 1T |
| Brass C260 | 0.8–1.5 | 0.5T | 1T | 1T |
| Brass C260 | 2.0–4.0 | 1T | 1.5T | 1.5T |
Mild Steel Baseline
Cold‑rolled mild steel is the most formable common sheet metal. For thicknesses up to 3 mm, 1T inside radius is comfortably achievable across the grain. For production reliability, specify 1.5T as your standard design radius.
6061‑T6 — Material Substitution Options
6061‑T6 has only 8–10% elongation vs. 25% for 5052‑H32. If your design requires tight‑radius bends, consider: switching to 5052‑H32 for better formability, using 6061‑T4 (annealed, then age after bending), specifying extruded profiles with formed features, or redesigning to avoid tight bends in T6 temper.
BEND RADIUS GUIDE
Understanding Bend Radius: Why the 1T Rule Matters
When you bend sheet metal, the outer surface stretches while the inner surface compresses. The tighter the inside radius, the more the outer fibers must elongate. If elongation exceeds the material’s ductility limit, cracks form. This is the physics behind every bend radius chart.
01
The 1T Rule — Rmin = K × T
Industry expresses minimum bend radius as a multiple of material thickness (T). Rmin = K × T, where K is a material factor based on ductility. Materials with high elongation get a low K; brittle or high‑strength materials get a high K. “1T” = inside radius equals material thickness. Always measured as inside radius (IR), not centerline or outside radius.
02
Material K‑Factors
Mild Steel CRS — K=1.0 (1T, baseline standard)
Stainless 304 — K=1.5 (work‑hardens during bending)
Aluminum 5052‑H32 — K=0.8–1.0 (excellent formability)
Aluminum 6061‑T6 — K=3.0–4.0 (low elongation, high cracking risk)
Copper C110 — K=0.5 (very ductile)
Brass C260 — K=0.5–1.0 (temper‑dependent)
03
Grain Direction — Why Orientation Changes Everything
Bending across the grain (perpendicular to rolling direction) allows a 25–50% tighter radius — fibers resist cracking independently. Bending with the grain (parallel) allows a single crack to propagate along an entire fiber. Practical rule: Always orient bends across the grain where possible. If bending both directions, design to with‑grain radius or specify grain direction on the drawing.
K‑Factor Reference — Inside Radius as Multiple of Thickness
A 2 mm material thickness means: 1T = 2 mm, 0.5T = 1 mm, 3T = 6 mm. Use this table to quickly determine your minimum radius for any material.
Mild Steel
K=1.0 · 1T
304 Stainless
K=1.5 · 1.5T
5052‑H32 Al
K=0.8–1.0 · 0.8–1T
6061‑T6 Al
K=3.0–4.0 · 3–4T
FORMING PHYSICS
Neutral Axis & Bend Allowance
The neutral axis is the plane within the bend where material neither stretches nor compresses. As the radius tightens, the neutral axis shifts inward, which is why bend deduction and bend allowance calculations must account for the actual inside radius, not a CAD‑default assumption.
| Material | K‑Factor | Rule of Thumb | Notes |
|---|---|---|---|
| Mild Steel CRS | 1.0 | 1T | Baseline standard |
| Stainless Steel 304 | 1.5 | 1.5T | Work‑hardens during bending |
| Aluminum 5052‑H32 | 0.8–1.0 | 1T | Excellent formability |
| Aluminum 6061‑T6 | 3.0–4.0 | 3T–4T | Low elongation, high cracking risk |
| Copper C110 | 0.5 | 0.5T | Very ductile |
| Brass C260 | 0.5–1.0 | 0.5T–1T | Temper‑dependent |
Practical rule: Always orient bends across the grain wherever possible. If your part requires bending in both directions (common on multi‑flange parts), design to the with‑grain radius for all bends, or specify the grain direction on the drawing so the fabricator can nest the part correctly.
The V‑Die to Bend Radius Relationship
On the shop floor, most bending is air bending on a press brake. In air bending, the inside radius is not determined by the punch nose radius — it is determined by the V‑die opening width. The relationship: R ≈ V / 6 (for mild steel). A 12 mm V‑die opening produces a natural inside radius of roughly 2 mm in mild steel. This is the practical bridge between your design specification and what actually happens on the machine.
| Material | Recommended V‑Die Opening | Expected Inside Radius |
|---|---|---|
| Mild Steel | 6–8 × T | ≈ V/6 |
| Stainless Steel 304 | 8–10 × T | ≈ V/6 to V/5 |
| Aluminum 5052‑H32 | 8–10 × T | ≈ V/6 |
| Aluminum 6061‑T6 | 10–12 × T | ≈ V/5 to V/4 |
Why wider V‑dies for aluminum and stainless? These materials have lower ductility (6061‑T6) or higher work‑hardening rates (304 SS) than mild steel. A wider V‑die produces a more gradual bend with less tensile stress on the outer fibers, which reduces cracking risk. The trade‑off: wider V‑dies require more tonnage for the same bend angle and produce larger natural radii. Always specify the die opening with your fabricator if the bend radius is critical to your design.
SHEET METAL FORMING GUIDE
Why Does 6061‑T6 Crack? Material Substitution Guide
The most common question: “My 6061‑T6 part keeps cracking at the bend. What can I do?” The answer is usually a material change, not a radius change. This guide covers the most common cracking scenarios and how to solve them.
Quick reference: 6061‑T6 has only 8–10% elongation vs. 25% for 5052‑H32. If it cracks, switch to 5052‑H32, use 6061‑O then re‑heat‑treat, or redesign to avoid tight bends. For stainless steel, use annealed tempers for better formability. Below are the specific substitutions for the most common scenarios.
Option 1
6061‑T6 → 5052‑H32
Problem: Cracking at bends below 3T.
Why it works: 25% elongation vs. 8–10%. Bends reliably at 1T.
Trade‑off: Lower UTS: 228 MPa vs. 310 MPa. Acceptable for most structural brackets, enclosures, and non‑critical applications.
Option 2
6061‑T6 → 6061‑O, Bend, Re‑Heat‑Treat
Problem: Needs 6061 strength + tight bends.
Why it works: Annealed 6061 bends at 1–1.5T. Heat‑treating after forming restores T6 properties.
Trade‑off: Adds process step and cost. Best for high‑value parts where 5052 is not strong enough.
Option 3
304 SS Half‑Hard → Annealed · 316 SS → 304 SS
304 SS Half‑Hard: Work‑hardening, inconsistent bends. Switch to 304 SS Annealed — softer temper bends more consistently at 1.5T (slightly lower yield strength).
316 SS: Requires very large radii (2T+). Switch to 304 SS — better formability (1.5T vs. 2T). Trade‑off: lower pitting corrosion resistance.
When to Machine Instead of Bend
For 6061‑T6 parts requiring radii tighter than 2T at thicknesses above 3 mm, CNC machining from plate is often the more reliable choice. The bend simply is not going to work, and trying to force it wastes material and machine time. Baetro offers both CNC machining and sheet metal bending; upload your CAD and our engineers will recommend the best process for your geometry and material.
5052‑H32
25% Elongation · 1T Bend
6061‑O + T6
1–1.5T Bend + Re‑Heat‑Treat
304 Annealed
1.5T Bend · Better Formability
BEND RADIUS FAQ
Frequently Asked Questions
The minimum bend radius is the tightest inside radius without cracking, expressed as a multiple of thickness (T). Mild steel ≈ 1T, 304 stainless ≈ 1.5T–2T, 6061‑T6 aluminum ≈ 3T–4T.
The 1T rule states the inside radius should be at least equal to thickness. It works for mild steel and 5052‑H32 aluminum — but not for 6061‑T6 or hardened stainless. The 1T rule is a starting point, not a universal law.
6061‑T6 has low elongation (8–10%) vs. 25% for 5052‑H32. When bent tight, outer fibers stretch beyond the limit and crack. Fixes: use a larger radius (3T+), bend across the grain, switch to 5052‑H32, anneal the bend zone then re‑heat‑treat to T6, or machine from plate instead of bending.
Grain direction matters significantly. Bending across the grain allows a 25–50% tighter radius than bending with the grain. Specify grain direction on drawings for critical bends.
For V‑die selection, in air bending: R ≈ V/6 (mild steel). For a 3 mm radius, use an ~18 mm V‑die. Wider dies (8T–10T) reduce cracking risk for aluminum and stainless. Radii requiring V‑dies narrower than 4T push into bottom‑bending territory with higher tonnage.
Bend radius directly determines bend allowance (arc length consumed in the bend) and influences K‑factor (neutral axis position). Tighter radii shift the neutral axis inward, producing a lower K‑factor. For flat‑pattern design: specify the inside radius first, then calculate bend allowance from there. Use your fabricator’s actual K‑factor values, not CAD software defaults, which often assume a radius‑to‑thickness ratio that doesn’t match your design.
Yes, and you should. Using a single consistent inside radius across all flanges eliminates tooling changes between bends, reduces setup time, and lowers part cost. Choose a radius that satisfies the tightest bend requirement on the part and apply it to all bends. The small increase in radius on less demanding flanges has no functional downside and makes the part faster and cheaper to produce.