Sheet metal face reference

Creates a sheet metal face by adding depth to a sketched profile. Feature shape is controlled by the sketch shape and any bends or seams between the new sheet metal face and existing sheet metal faces.

Access:

Ribbon: Sheet Metal tab Create panel Face

The Face dialog box has three tabs that select and define the face you are creating.

Shape

This tab controls the selection of sheet metal faces and the bend settings to use when joining two or more faces.
Shape
	Selects one or more profiles to extrude by the sheet metal thickness.
	Single profile Automatically selects profile and previews the sheet metal face.
	Multiple profiles Position the cursor over the profile and click to select. To cancel the selection, press Ctrl and click profile.
	Click Offset to change the direction of the extrusion.

Bend
Bend radius	The default bend radius is displayed. Click the down arrow to select from other options: Measure uses a measuring command to calculate the bend radius value. Show Dimensions displays dimension values. Click to add as the bend radius value. List Parameters shows parameters associated with the model. Click to select and enter a parameter name in the Radius field.
	Edges - select additional sheet metal face edges to include in the bend.
	For a new sheet metal face, you can create a bend to an existing sheet metal face. Select the sheet metal edge for the bend if one of the following applies: The profile for the new sheet metal face overlaps with multiple existing sheet metal edges. The profile for the new sheet metal face does not overlap any sheet metal edges. Autodesk Inventor trims or extends the sheet metal faces as required to create the bends.

Bend Extension

Click here to review the material on Bend Extension that is common to: Bend, Face, and Contour Flange features.

Unfold Options tab

For information about the Unfold Options tab, see the Sheet metal unfold options reference.

Bend tab

For information about the Bend tab, see the Bend Relief Options reference.

OK	Click OK to create (or modify) a face using the parameters and options specified and close the dialog box.

Apply

Click Apply to create a face using the parameters and options specified and leave the dialog box open allowing the creation of additional faces using other available sketches.

Cancel

Click Cancel to discard any edits made to parameters or options and close the dialog box.

(More)

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.

	Fix Edges	Equal bends are added to the existing sheet metal edges.
	45 Degree	Sheet metal faces are trimmed or extended as necessary and 45 degree bends are inserted.
	Full Radius	Sheet metal faces are trimmed or extended as necessary and a full radius (half-circle) bend is inserted.
	90 Degree	Sheet metal faces are trimmed or extended as necessary and 90 degree bends are inserted.
		Flip Fixed Edge - By default, for 45 Degree, Full Radius or 90 Degree bends, the first selected edge is fixed and the matched edge (highlighted in red on the new face) is trimmed or extended, if necessary. Select Flip Fixed Edge to reverse the order.