Use the Bend Part command to bend a portion of a part.
First, you define the location of the bend, then you specify the side of the part to bend, the direction and other parameters of the bend.
To define the bend line, or the location of the bend, use a sketch of an open profile consisting of a single line segment. The plane on which the sketch is created serves as the neutral plane of the bend. It’s good practice to place the sketch plane on the side of the part where the bend occurs or at the center of the bend. Also, place your sketch plane at a height where you can measure the results.
Also, you can limit the length of the open profile so that it touches only the portion of the part that you want to bend. Sketch the open profile directly on the face of the portion you want to bend. Then, bend one portion of the part rather than multiple portions that can lie on the same projection direction of the open profile.
Bend Part requires both a consumed sketch, such as an extruded face, and a sketch that is visible and unadaptive (such as a line sketched across the extruded face).
- Click 3D Model tab
Modify panel Bend Part 
. - Use the Bend Line selector in the Bend Part dialog box to select the line about which the feature hinges or folds.
- Click the pop-up menu and choose how you want to define the bend:
- Radius + Angle. Creates a feature using a radius and angle that you specify. The radius defines the size of the bend curve between the two sides. The angle defines the position of the two sides.
- Radius + Arc Length. Creates a feature using a radius and arc length that you specify. Arc Length defines the length of the curve.
- Arc Length + Angle. Creates a feature using values you specify for Arc Length and Angle. The Arc Length defines the length of the curve. The angle defines the position of the two sides.
- Choose whether the part bends left, right, or both ways around the bend line.
- (Optional) Click Direction to change the side of the part on which the bend occurs. Tip: If the Bend Line intersects multiple portions of the part body, select Bend Minimum to specify which portions to bend.
- Click OK.