To Work with Faces in Sheet Metal

You use Face to create a face from a sketched profile. (You can use a shared sketch as a profile.)

What's New: 2019

The sketch shape and any bends or seams between a new sheet metal face and existing sheet metal faces control the shape. If desired, you can use a shared sketch as a profile for a face.

You can also override default sheet metal styles in the Face dialog box as you create your sheet metal face. These settings include how the flat pattern unfolds, and the bend relief settings between faces.

Create a 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.

1. Sketch a profile that represents the shape of the sheet metal face you want to create.
2. On the ribbon, click Sheet Metal tab Create panel Face .
3. If there are multiple profiles, click Profile and then select a profile for the sheet metal face.
4. If there are two or more solid bodies in the part file, click the Solids selector to choose the participating solid body.
5. (Optional) If a body exists, click New Solid to create a new body.
6. To change the direction for the thickness of the face, click a selection in Offset Direction.
   • Click Flip Side or to offset the material thickness to the other side of the selected profile.
   • Click Both Sides to offset the material thickness equally to both sides of the selected profile.
7. (Optional) Do one of the following:
   • Select the Follow Defaults checkbox to link the material thickness and rules to the Default setting.
   • Clear the Follow Defaults checkbox and click the drop-list to specify a unique material thickness and rules from the predefined list.
8. Do one of the following:
   • Click OK to create the face and close.
   • Click Apply if you want to create more sheet metal faces.

Specify Bend and Fold for Faces

The Shape tab lets you specify the sheet metal faces and the bend settings to use when joining two or more faces. Faces are automatically trimmed or extended to create the bend.

Single bends are created by default when you use the Face command. Selecting More provides options to define double bends. The options are not available for base features.

1. In the Radius drop-down list, do one of the following to specify the bend radius:
   • 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.
2. 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.
3. To extend material along the faces on the side of the edges connected by the bend, click Extend Bend Aligned to Side Faces.
4. 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 Bend Extension reference to review the material on Bend Extension that is common to: Bend, Face, and Contour Flange features.
5. (Optional) 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: 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.

Use a Shared Sketch as a Profile for a Face

• 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.