Sheet metal bending

Sheet metal bending (also called press braking or brake forming) is a forming process that permanently deforms sheet metal along a straight bend line. It is usually done on a CNC press brake, where the upper tool (the punch) presses the sheet into the lower tool (a die with a V opening), and it typically follows laser cutting of the flat pattern.

Bending stretches the outside of the material and compresses the inside. The neutral axis between them keeps its length, and the flat pattern is calculated from it. Its position is expressed by the K-factor, usually between 0.3 and 0.5, which depends on the material, the ratio of bend radius to thickness and the tooling; CAD uses it to derive the bend allowance or bend deduction.

The most common method is air bending: punch depth sets the angle, so one tool set can produce different angles. On release, the sheet partially springs back (springback), which the press brake compensates for by overbending; modern machines also measure the angle during the bend. Bottoming or coining needs more force but gives a more accurate angle. Long, simple bends can also be made on swivel-beam folding machines, and series production uses automatic panel benders.

The V-die opening is usually 6 to 10 times the sheet thickness. The inside bend radius in mild steel then comes out at about 15 to 17% of the die opening, roughly one to one and a half times the thickness. The minimum flange length is about 0.7 times the die opening, or as a rule of thumb 4 to 7 sheet thicknesses. Typical accuracy is about ±0.5 to 1° on the angle and a few tenths of a millimeter on dimensions across a bend.

Sheet metal bending is the cheapest route to enclosures, covers, frames, brackets, mounts, profiles and channels, from one-offs to medium volumes. It needs no part-specific tooling, since the press brake uses standard punches and dies, so the prototype and the production part can be made the same way. A bent part is usually lighter and cheaper than a milled part with the same function and can often replace a weldment.

For very large runs with embossed and formed features, stamping in a progressive die can be more economical. Complex shapes with varying wall thickness are the domain of castings and machining.

Holes and cutouts too close to a bend distort, so as a guideline keep them at least two to three sheet thicknesses from where the bend starts. Where a bend ends at the edge of the sheet, add a bend relief at least as wide as the sheet is thick, or the corner will tear. A bend line parallel to the rolling direction is more prone to cracking. Hard aluminum alloys in the T6 temper (such as EN AW-6082) crack at small radii, and alloys such as EN AW-5754 suit bent parts better (in North America, 6061-T6 behaves similarly and 5052 is the usual choice). Stainless steel and high-strength steels spring back considerably more than mild steel.

CAD calculates the flat pattern with a K-factor that may not match a given fabricator's tooling. Supply both a 3D model and a drawing, and agree on who prepares the flat pattern and whose values apply. Dimension the functional features and remember that tolerances stack up across multiple bends. Check that the bends can be made in the planned sequence without the part hitting the tooling or the machine. For cosmetic parts in stainless steel, aluminum or pre-painted sheet, ask for mark-free bending, for example through a protective film.