Minimum Bend Radius Chart for Sheet Metal

Recommended Starting Inside Bend Radius

Material	Sheet Thickness	Recommended Starting Inside Radius
Mild steel / cold-rolled steel	1–6 mm	1 × T
Mild steel / cold-rolled steel	6–12 mm	1–1.5 × T
Stainless steel 304	1–6 mm	1.5–2 × T
Stainless steel 304	6–12 mm	2–3 × T
Aluminum 5052-H32	1–6 mm	1 × T
Aluminum 5052-H32	6–12 mm	1.5 × T or more
Aluminum 6061-T6	1–6 mm	3–4 × T
Aluminum 6061-T6	6–12 mm	4 × T or more

T = material thickness
R = inside bend radius

Important: Minimum in this page title means a practical DFM guideline. It does not mean every press brake, die set, material condition, or fabricator can produce the listed radius in every situation.

Material-Specific Bend Radius Guidelines

Material	Recommended Starting Radius	Design Notes
Cold-rolled steel	1 × T	Suitable starting point for standard brackets, covers, and enclosures
Galvanized steel	1–1.5 × T	Use a larger radius if zinc-coating cracking or cosmetic damage is unacceptable
Stainless steel 304	1.5–2 × T	Higher springback; increase radius for thicker sheet, hard tempers, or cosmetic surfaces
Aluminum 5052-H32	1 × T	Good formability; commonly used for bent enclosures and fabricated parts
Aluminum 6061-T6	3–4 × T	Higher crack risk; avoid sharp bends unless validated by material condition and process
Aluminum 6061-O	1–1.5 × T	Annealed aluminum bends more easily than T6 material
Copper C110	1–1.5 × T	Annealed aluminum bends more easily than T6 material
Brass	1–2 × T	Depends strongly on alloy, temper, and bend direction

Do not specify only aluminum when bend radius is important. Aluminum 5052-H32 and 6061-T6 have very different forming behavior, as 5052-H32 is generally more suitable for formed parts, while 6061-T6 usually needs a larger radius and closer process review.

Rounded Starting Examples by Thickness

Use these as early design references. Final bend radius should be confirmed against the selected material condition, bending method, available tooling, and cosmetic requirements.

Sheet Thickness	CRS / Mild Steel	304 Stainless Steel	Aluminum 5052-H32	Aluminum 6061-T6
0.8 mm	R0.8 mm	R1.5 mm	R0.8 mm	R2.5–3.0 mm
1.0 mm	R1.0 mm	R1.5–2.0 mm	R1.0 mm	R3.0–4.0 mm
1.2 mm	R1.2 mm	R2.0–2.5 mm	R1.2 mm	R4.0–5.0 mm
1.5 mm	R1.5 mm	R2.5–3.0 mm	R1.5 mm	R4.5–6.0 mm
2.0 mm	R2.0 mm	R3.0–4.0 mm	R2.0 mm	R6.0–8.0 mm
2.5 mm	R2.5 mm	R4.0–5.0 mm	R2.5 mm	R8.0–10.0 mm
3.0 mm	R3.0 mm	R4.5–6.0 mm	R3.0 mm	R9.0–12.0 mm
4.0 mm	R4.0–6.0 mm	R6.0–8.0 mm	R4.0 mm	R12.0–16.0 mm
5.0 mm	R5.0–7.5 mm	R7.5–10.0 mm	R5.0 mm	R15.0–20.0 mm
6.0 mm	R6.0–9.0 mm	R9.0–12.0 mm	R9.0 mm	R24.0 mm or more

Why Bend Radius Matters

A radius that is too small stretches the outside surface of a bend beyond what the material can safely accommodate. This can cause:

Cracks along the outside bend surface
Coating damage or zinc-layer cracking
Visible whitening, crazing, or fracture in aluminum
Reduced fatigue life in the bend area
Inconsistent bend angles and springback
Higher forming force and possible tooling damage

A larger bend radius reduces strain and crack risk, but it also affects bend allowance, flat-pattern dimensions, enclosure clearances, and final formed geometry.

Why Tooling Changes the Radius

In air bending, the finished inside radius is not controlled only by the punch tip. Material properties, thickness, V-die opening, bend angle, and press-brake setup all influence the final formed radius.

Tooling Factor	Effect on the Bend
Larger V-die opening	Usually produces a larger inside bend radius
Smaller V-die opening	Can produce a tighter radius but requires more forming force
Larger punch nose radius	Can reduce sharp-bend strain when compatible with the die opening and forming method
Material hardness	Increases springback and may require a larger radius
Material thickness	Usually requires a larger die opening and bend radius
Bottoming or coining	Can form tighter radii but needs higher tonnage and suitable tooling

Do not assume that a radius shown on a drawing can be achieved exactly with standard air-bending tools. Confirm available punch and die combinations when radius affects fit, sealing, appearance, or a mating interface.

Radius Affects Bend Allowance

Bend radius changes the material length consumed in the bend. For a given angle:

A larger inside radius increases bend allowance
A different K-factor changes the neutral-axis location
Material, thickness, tooling, and bending method affect developed length

The standard bend allowance equation is:

BA=π180×A×(R+K×T)BA = \frac{\pi}{180} \times A \times (R + K \times T)BA=180π×A×(R+K×T)

Where:

BABABA = Bend allowance
AAA = Bend angle in degrees
RRR = Inside bend radius
KKK = K-factor
TTT = Material thickness

Use your fabricator’s validated bend table instead of a generic K-factor when flat-pattern accuracy is important.

Internal link: Sheet Metal Bend Allowance and Bend Deduction Chart

Checks Before Releasing a Drawing

Match bend radius to the exact material grade and temper, not only the material family
Use at least 1 × T when material details are unknown
Use larger radii for stainless steel, high-strength steel, and heat-treated aluminum
Place tight bend lines perpendicular to rolling direction whenever practical
Keep holes, slots, cutouts, and self-clinching hardware outside the bend deformation zone
Avoid locating cosmetic surfaces on the outside of tight bends where cracking or marks are unacceptable
Specify material grade, temper, thickness, bend direction, and inside radius when they are functionally critical
Request a first-article sample for tight-radius, cosmetic, structural, or high-load bends

When a Small Radius Is Required

If the design needs a radius below the normal recommendation, consider the following options.

Option	When It Helps	Trade-Off
Use a more ductile material	Tight bends in aluminum or stainless parts	May change strength, corrosion resistance, availability, or cost
Specify annealed material	Tight bends in aluminum or copper	May reduce strength or hardness
Increase bend radius	Cracking or cosmetic damage is a concern	Changes formed geometry and flat-pattern dimensions
Bend perpendicular to rolling direction	Material grain direction is known	May affect nesting efficiency and material use
Add bend reliefs	Bend ends near an edge, slot, or cutout	Adds features and may affect appearance
Use a forming tool or staged operation	Tight local geometry is essential	Increases setup, tooling, and cost
Machine a relief groove before forming	Very tight or controlled bends are required	Reduces local section strength and adds processing

Do not specify a very small bend radius without identifying the actual material and temper. A bend that works in 5052-H32 may crack in 6061-T6 even when thickness and nominal radius are the same.

Frequently Asked Questions

Learn how to choose the right sheet metal bend radius for different materials, including mild steel, stainless steel, and aluminum. Understand how thickness, material properties, and rolling direction affect bending performance and part quality.

What is the minimum bend radius for sheet metal?

A practical starting point is an inside bend radius equal to material thickness, or R=1×TR = 1 \times TR=1×T. The safe radius changes with material grade, temper, thickness, rolling direction, bend angle, and tooling.

What bend radius should I use for mild steel?

For common cold-rolled or mild steel, start around 1 × material thickness. For thicker material, long bends, or more demanding cosmetic requirements, use 1–1.5 × thickness and confirm the final tooling setup.

What bend radius should I use for stainless steel?

For 304 stainless steel, start around 1.5–2 × material thickness for thin sheet. Use 2–3 × thickness for heavier gauges, hard tempers, tight cosmetic requirements, or bends that must run parallel to the rolling direction.

What bend radius should I use for aluminum?

Aluminum 5052-H32 commonly starts around 1 × material thickness. Aluminum 6061-T6 is less forgiving and should generally start around 3–4 × thickness, with larger radii for heavier sheet or crack-sensitive bends.

Does rolling direction affect bend radius?

Yes. Tight bends have a higher crack risk when the bend line is parallel to the sheet’s rolling direction. Place the bend line perpendicular to rolling direction whenever practical, or increase the radius.

Need Help Validating Your Sheet Metal Bend Design?

Upload your CAD files and our engineers will review bend radius, material selection, and DFM requirements to help prevent cracking, rework, and production issues.

Capabilities

Fabrication

Value-Added

3D Printing

Material

Products

Sheet Metal Parts

Thermal & Electrical

Sheet Metal Enclosure

Energy & Infrastructure

Industries

Resource

Why Choose Us