Bending is not an option for 6061 Aluminum or PCM metals. At this time bent parts cannot also be engraved.

You have two options when ordering bent parts - 2D or 3D.

Upload a STEP file with bent parts - the site will unfold them for you.

Use different color lines in your 2D vector ‘dxf’ ‘ai’, ‘eps’ or ‘svg’ design file for bending and cutting. Eg In the screenshot below, blue and red are assigned to cutting and green to bending.

Optional: After ordering, you are welcome to reply to your order confirmation email with a 3d rendering of your part to help the team better understand your desired results.

The bend angle is measured on the outside of the bend. The maximum bend angle is 130° (50° on the inside of the bend, or acute side). The minimum bend angle is 5° (175° on the inside of the bend, or obtuse side).

Window & joggle bends are allowed, up to 90°.

At this time we cannot offer curl, bump, or roll forming, coining, or hemming.

For channel bends, the base must be at least 2 times wider than the flange length. The base can be greater than 2:1. For example, a 5” base with 1” flanges is fine (that would be a 5:1 ratio).

For box bends (where there are two sets of parallel opposing bend lines, on opposite sides of a rhombus base) there is a maximum flange length of 3.50" (88.9mm).

See materials pages and the full laser cut metals design guide.

Listed on our metals materials pages under ‘bend parameters’ these numbers can be incorporated into your design process to help ensure final part dimensions meet your needs.

K-factor is the ratio between the "neutral axis" of a bent part and the thickness of the material. The "neutral axis" is where the material doesn't elongate or compress during the bend. The bend deduction is the compensation value for the amount the material will stretch when bending your part .These values are specific to each material type, thickness, and bend angle.

We recommend using 3D CAD software to design metal parts, so you do not have to worry about manually calculating bend deductions. You can tell your software what k-factor and bend radius to use for the material, and it will automatically create the correct flat pattern size and bend locations so that the finished part size after bending matches your design. You can find the K-factor values and bend radius for each material on the materials pages.

When metal is bent there is a slight bulge of material at the ends of the bend. It is common to include some bend relief notches (small semi-circles) to mitigate the effect of the bulge.

The width of the bend relief notches should be 50% of material thickness at 90 degrees. The depth of the notches should be the material thickness plus the bend radius, plus an added 0.02"/0.5mm for safety's sake, at minimum. Your CAD software should have a tool to add relief notches into your design.

All bend lines must be parallel to a straight part edge so that there is a reference surface to position the part for bending. This is called a "gauging edge".

If you wish to have an irregular flange shape, you'll need to add a tabbed bend surface to provide a parallel gauging edge.

EG To make a part such as this:

You'll need to submit a file with the irregular path tabbed and an additional square section added.

Sheet metal is formed using a punch and die. The metal part is placed between a punch and a V-die as shown below:

The press brake forces the punch and the die together and the metal folds where the punch makes contact with the part. The part itself only touches the punch on the bend line and the die on the edges.

As a result of the above process, marks from the bending process will be visible. Your part will have marks where the metal touches the punch and die.

The bend radius is the radius of the bent metal where the punch meets the part. Exact 90-degree angles are not possible to manufacture so there will always be a radius on the bend.