Fold sheet metal bodies

Fold (also known as Bend) folds a sheet metal body along straight sketch lines. Learn how to use the Fold tool in Fusion.

Before you can fold a sheet metal body, create a sketch on the face of the sheet metal flange and position a straight sketch line for each fold.

1. On the Sheet Metal tab, select Create > Fold .

   The Fold dialog displays.

2. In the canvas, select a face to be the Stationary Side.

3. Select straight sketch lines that are planar to the Stationary Side to fold.

   Note: The order of selecting the bend lines is important. To bend a sheet metal body across several lines, start with the lines farthest from the stationary side.

4. Specify the Bend Angle relative to the stationary side.

   The angle cannot be 0 and must be greater than -180 or less than 180 degrees.

5. Optional: In the Fold dialog, adjust the options and associated settings for each fold:

   • Flip : Flips the direction of the bend.
   • Bend Line Position : Specifies the location of the bend.
     • Start : Starts the bend at the sketch line.
     • Center : Centers the bend on the sketch line.
     • End : Ends the bend at the sketch line.
   • Bend Relief:
     • On: Automatically applies a bend relief where necessary. If Bend Relief is turned on, you can use the Override Rules to create different bend relief shapes.
     • Off: Disables bend reliefs for the bend.

6. Optional: In the Fold dialog, adjust settings:

   • Corner Relief: Check to automatically apply a corner relief where necessary. Uncheck for no corner reliefs.
   • Override Rules: Check to override the the bend, bend relief and corner relief options.

7. Click OK.

The sheet metal body with specified bends displays in the canvas.