Aluminium sheet metal bending guidelines for 5052 and 6061

Aluminium does not bend like steel, and the difference shows up as a crack on the outside fibre of the first production part rather than as a warning at the design stage. The two numbers that decide it are the inside radius relative to thickness and the springback angle after the punch releases. Get those wrong on 6061-T6 and a 1t radius that looks generous on a steel drawing will crack every part in the batch.

These aluminium sheet metal bending guidelines cover press-brake forming of aluminium sheet from 1 mm to 6 mm in the alloys a canopy, rack, enclosure or vehicle panel is likely to use. Stamping and deep drawing of aluminium is a separate problem, covered in aluminium stamping formability and tooling, and cutting is covered in laser cutting aluminium sheet and plate. This page is about the bend. It belongs to the bending, welding and assembly guides.

What radius does aluminium need at 90°?

The minimum inside radius for a 90° bend is 1t in 5052-H32, 1.5t in 6061-T4 and 2.5t to 3t in 6061-T6, measured across the rolling direction. Turn the bend line to run along the rolling direction and the usable radius roughly doubles; that orientation is the worst case, because the elongated grain boundaries that form during rolling lie parallel to the bend line and separate under tension.

The mechanism is elongation. A 90° bend with an inside radius of 1t stretches the outside fibre by about 33%, calculated as (R + t) / (R + 0.5t) − 1. 5052-H32 has 12–15% elongation, which is why 1t works only when the grain runs across the bend. 6061-T6 has 8–10%, so 1t demands more strain than the alloy has and the outer fibre tears within a few degrees of the punch contacting.

Three shop rules make the difference between a forming operation and a crack:

• Keep the punch nose radius at 1.5t or larger. A sharp punch concentrates strain at the bend line.
• Deburr laser-cut edges before bending. Dross and a hard oxide edge act as crack starters.
• Place the bend line across the rolling direction unless the drawing forces otherwise, and mark the grain direction on the drawing.

Springback: the angle you program is not the angle you get

Aluminium's modulus is about 69 GPa against 210 GPa for mild steel, so it recovers roughly three times as much elastic strain. In practice, a 2 mm 5052-H32 part bent to 90° springs back 4–6°, and a 2 mm 6061-T6 part springs back 10–14°. That is the difference between a lid that sits flat and one that stands 3 mm proud at the corner.

The correction is overbending: program 96° to leave 90° in 5052, and 102–104° to leave 90° in 6061-T6. A CNC brake stores this per bend, which is why the same part run on a manual machine by a different operator comes out at a different angle. The 5-axis control on our brake holds the correction in the programme rather than in the operator's wrist.

Springback also varies with the die opening and the radius. A wider V die reduces the forming force and increases recovery; bottoming the punch into the material reduces it and marks the part. For aluminium, most production work is air bent with a corrected angle, not bottomed.

Aluminium sheet metal bending guidelines: alloy, radius and springback

The table gives working values for a 90° bend with the bend line across the rolling direction. Springback figures are for 2 mm sheet after release, measured on the part, not on the control.

Values move with thickness and with the actual mill certificate. A 3 mm 5052-H32 sheet at 1t behaves better than a 1 mm sheet at the same ratio, because the thinner sheet has less material to distribute the strain and a proportionally larger burr.

The flat pattern: K-factor for aluminium

K-factor for aluminium air bending sits around 0.42–0.46, close to but not identical to mild steel. Using the bend allowance formula BA = 0.01745 × A × (R + Kt), a 2 mm 5052-H32 part with a 2 mm inside radius and K = 0.44 gives:

• BA = 0.01745 × 90 × (2 + 0.88) = 4.52 mm per bend
• Bend deduction = 2 × (2 + 2) × tan 45° − 4.52 = 3.48 mm
• Six 90° bends: 20.9 mm consumed from the blank

Shift K to 0.50, which is what happens when a supplier assumes steel rules, and the deduction falls to 3.29 mm — 1.1 mm less over six bends. On a 1,200 mm cover that error lands on the last flange and shows as a gap.

Two habits prevent it. Dimension every flange from one bend origin instead of chaining dimensions, and ask for the K-factor and the die opening in the quotation. How to calculate bend allowance shows the derivation, and the bend allowance calculator will run the numbers for a specific alloy.

Die selection and the tooling that marks aluminium

Aluminium is soft enough that the die leaves a record of every setup. The V-die opening for aluminium should be 10t to 12t, wider than the 8t used for mild steel, for three reasons: it reduces the forming force, it lowers the strain at the bend line because the radius is larger relative to thickness, and it keeps the punch nose off the visible face. A 2 mm aluminium part on a 16 mm die forms a radius near 2.6 mm; on a 24 mm die it forms near 3.8 mm, which clears the 1t minimum for 5052 comfortably and still falls short of the 5 mm that 2 mm 6061-T6 needs.

Marks come from three places: the punch nose, the die shoulders, and the operator's gloves. Polished tooling and a protective film handle the first two. Film on both faces is the usual protection for visible aluminium panels, and it comes off before pretreatment. Glove marks on mill-finish aluminium do not come off at all, because the surface oxide traps the oils.

Galling is the other tooling failure. Aluminium picks up on an unpolished punch and transfers, leaving a rough streak along the bend that reappears on every part. Once a punch has picked up, it needs polishing before the next run; no amount of lubricant fixes a tool that has already started to transfer.

Welding, coating and the strength you lose at the bend

Bending 6061-T6 and then welding it creates a heat-affected zone where strength drops by roughly 30–40% in the as-welded condition. If the part is structural, the sequence should be: bend in T4, weld, then age to T6. If the drawing says T6 and the part is welded, the temper on the finished assembly is not T6 at the weld, whatever the certificate says.

Coating aluminium needs a conversion coating before powder. The oxide that forms naturally in air is not a paint base; a chromate-free conversion layer in the pretreatment line is. Cure cycles at 180–200 °C are safe for 5052 and cause slight overage in 6061-T6, which matters only where the part is designed to the minimum T6 properties. Degreasing before powder coating covers the cleaning stage that has to come before any conversion coating will hold.

Bent aluminium also work-hardens. A part bent twice in the same direction at a 1t radius is closer to H34 than H32 at the second bend, and the second bend is where the crack appears. If a drawing has two bends close together, increase both radii or anneal between operations.

How to inspect a bent aluminium part

First-off inspection for aluminium adds two checks that a steel part does not need. Check the outside fibre of every bend under 10× magnification for a crack or an orange-peel texture; a crack starts at the edge of the blank and runs inward along the bend line, so inspect within 20 mm of each edge first. Then check the angle with a digital protractor at both ends of the bend, because springback on a 4,450 mm part is not uniform along the length.

Radius is checked with a radius gauge on the inside of the bend, not calculated from the die. A 2 mm 5052 part that should read R2 and reads R2.8 tells you the die opening was wider than the quotation assumed, which is useful information before the next 500 pieces are cut.

Flatness matters on aluminium covers because the material is less stiff than steel: a 1.5 mm 5052 cover at 1,200 mm × 600 mm will show 3–4 mm of bow from its own weight if it is stacked flat before packing. Inspect it standing or on edge, and pack it that way.

What Ganesh runs

Aluminium blanks come off the 12 kW fibre laser, or one of the two 6 kW and two 3 kW support machines, on a 40 ft × 16 ft working area — long enough that a canopy skin or rack side is a single piece with a clean edge before forming. Press work is on our 200 T 5-axis brake, 4,450 mm of bed, Delem control, 10 mm maximum thickness, with springback correction stored per bend. Aluminium sits in the material list alongside CRCA, mild steel, stainless, brass and copper.

Welded parts go to the CLOOS robotic cells or to the manual MIG, spot and SPM stations — more than 30 of them — and the fixtures come out of our own tool room. Coating is in-house: seven-tank pretreatment, shot blasting where specified, an 18 ft × 14 ft powder booth and a curing oven, with DFT and cross-hatch adhesion checked in process. General tolerance is ±0.5 mm with closer limits by agreement; the plants run to ISO 9001:2015 and ISO 14001:2015.

What to put on the aluminium drawing

1. Alloy and temper separately — "6061-T6" is two specifications, and the temper drives the radius.
2. Thickness with a tolerance, and the mill certificate requirement if the part is structural.
3. Inside radius per bend, with a note if it is a maximum as well as a minimum.
4. Bend direction relative to the rolling direction, or the grain direction marked on the blank.
5. Bend line table with angle, direction and tolerance; state whether the angle is measured before or after springback.
6. Visible faces and the acceptable mark pattern, including glove and die marks.
7. Whether the part is welded after bending, and the temper required after welding.
8. Surface treatment: conversion coating, powder or anodising, and the masking areas for earthing.

When aluminium is the wrong choice

If the bend radius the design needs is below 1t and the load path is structural, aluminium is the wrong material; mild steel or stainless will form there and aluminium will crack. If the part is a load-bearing rack upright, 2 mm CRCA at 1.5t is cheaper per unit of stiffness than 3 mm aluminium, because aluminium's modulus is a third of steel's. If the part needs to be anodised after forming, check that the bend does not open the grain structure in a way that shows as a lighter streak on the anodised face.

If the geometry is a deep drawn cup rather than a folded panel, the route is stamping, not bending, and the aluminium stamping note is the relevant scope. If the panel is stainless, the surface-damage rules differ again and bending stainless steel without surface damage covers them.

Send the drawing with alloy, temper, thickness and the bend table. Our engineering team checks the radius against the die opening and the springback correction before quoting, so a crack at first-off is a design conversation rather than a rejected batch. Bending capability detail is on the CNC press brake page; start the route at request a quote.