Sheet Metal Bending

If you're designing parts using 3D CAD sheet metal features, please read and understand the following practical considerations. (If we're doing your 3D sheet metal CAD from a paper sketch, we'll deal with this.)

General bending considerations:

In general, parts should be designed with a 1T bend radius - radius equal to the sheet thickness - for the simplest setup, and to ensure we can form the intended geometry. In general, mild steel, type 304 stainless sheet, and thin, soft aluminum up to 1/8" thick can be formed at 1T without further considerations.

Sharper bends are possible - this may either expand or limit your options depending on the situation. Sharper bends enable designing with narrower edge flanges, and features closer to bend lines.

Aluminum may require a larger bend radius (e.g. 1.5T or more) to avoid cracking - please refer to our Minimum Bend Radius Chart and Gauge Chart. In general where bending aluminum is required, we recommend 5052-H32, other considerations notwithstanding.

When forming in our press brake, the exact radius formed is a complex function of the material type, thickness, the punch (upper tool) radius and the vee (lower tool) width. If your application requires high precision bends, it's most efficient to contact us with your requirements and have us recommend a bend radius to use in your models, based on the specific tooling to be used.

Large radius bends:

Larger radius bends are possible - often for aesthetic product design, or simply for function, metal needs to be bent at a far larger radius. Precise, simple bend setups are routine up to 1/2" radius as they are generally done in a single hit using hard tooling. While we can handle anything, it's most cost-effective to draw radii that match our tooling: 3/16", 1/4", 3/8", 1/2" radius, and also 3/4" and 1" although the bending method may differ.

Forming even larger radii, e.g. 2", or 6", is done using precisely-located multiple hits - called bump forming. We do this routinely, but it adds to the cost, and may require cutting additional setup parts to dial in the settings.

Bending geometry limitations:

We bend using a press brake, which in general pushes a vee shaped punch into a vee shaped die, with the material lifting an equal amount on each side of the die. For a 90 degree bend, the material on either side of the bend lifts 45 degrees.

The vee die is selected to match the material thickness and bend radius, and so the vee imposes a minimum flange width (distance from bend to part edge). If the bend is too close to the part edge, the part edge drops into the die before the bend is fully formed, most likely resulting in the bend ending up in the wrong location. Holes and other cut features closer to the bend line than the minimum flange width may not form as expected. In general the minimum flange width is 4 to 5 times the bend radius. See Minimum Flange Widths

The material can't be in the same place as the punch, die, or upper or lower ram of the press brake. For parts with more than one bend, the bend order is planned to ensure the part can fit in the die, the die can close, and the part can swing as needed, without the part colliding with anything.

There are some fundamental limitations. Parts with two 90 deg bends forming a "U" shape can be formed only when the bottom of the "U" is at least as wide as the shorter of the two sides of the "U". For larger parts, the bottom may need to be at least 1" wider than the shorter side.

Deep boxes, i.e. parts with flanges folded up on all 4 sides, can't be deeper than about 2-1/2", or the already-bent adjacent sides collide with the brake upper ram.

Metal doesn't magically follow the shape of the punch and die - it's best to have a symmetric shape of metal within the 1/2" or so on either side of the bend line, otherwise the actual bend location tends to drift based on the path of least resistance. For best results, part edges that cross bend lines should cross perpendicular to the bend, and extend symmetrically by a distance of at least the minimum flange width.

Reverse flanges, i.e. where the sheet bend one way and then the other, also have restrictions. Parallel reverse bends must be far enough apart for the already-formed bend to not collide with the vee die when making the second bend. Perpendicular reverse bends, e.g. forming a saddle shape, may collide with the lower ram.

It helps to understand the general geometry limitations. We'll advise based on your specific design.