Create sheet metal face

Add thickness to a sketch profile to create a sheet metal face.

The first feature that you create is the base feature. For subsequent sheet metal faces, when one line in the profile is coincident with an existing sheet metal edge, a bend is created automatically.

Note: Bend and edge options are not available for the base feature.

To begin, sketch a profile that represents the shape of the sheet metal face you want to create.

1. On the ribbon, click Sheet Metal tab Create panel Face .

   If there is only one profile in the sketch, it highlights.

2. If there are multiple profiles, click Profile and then select a profile for the sheet metal face.
3. To change the direction for the thickness of the face, click Offset.
4. Click OK to create the face and close,

   or, to create additional sheet metal faces, click Apply.

5. Accept the default bend radius specified in the active sheet metal style, enter a value, or on the drop-down list, select Measure, Show Dimensions, or List Parameters to enter a different value.
6. If the profile is not coincident with an existing edge, or if more than one line in the profile is coincident with an existing face, select an edge to create the bend. Select parallel edges to create a bend.

   Faces are automatically trimmed or extended to create the bend.

7. To extend material along the faces on the side of the edges connected by the bend, click Extend Bend Aligned to Side Faces.
8. If sheet metal faces are parallel but not coplanar, click an edge on the existing face (where the bend joins). Then click More, and specify a method for creating a Double Bend between the sheet metal faces. See the Bends dialog box for an explanation of the methods.
9. Optionally, click Flip Fixed Edge to trim or extend the selected edge while the matched edge is fixed. When not selected, the order is reversed.

Note: You can use a shared sketch as a profile. In the browser, click the plus sign beside the feature that contains the sketch you want to use, right-click the sketch icon, and then select Share Sketch.

Note: If the default bend or fold settings are not appropriate, override the values for an individual face feature using the Unfold Options tab or the Bend tab.