Create sheet metal face

Create a sheet metal face by adding thickness to a sketched profile. If it is the first feature created, it 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.

Create first sheet metal face

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 is automatically highlighted.
  2. If there are multiple profiles, click Profile and then select the profile for the sheet metal face.
  3. Click Offset to change the direction for the thickness of the face.
  4. Click OK. Optionally, click Apply to create the face and keep the dialog open to create additional faces.
Note: Bend and edge options are not available for the base feature.

Create additional sheet metal faces

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 is automatically highlighted.
  2. If there are multiple profiles, click Profile and then select the profile for the sheet metal face.
  3. Click Offset to change the direction for the thickness of the face.
  4. Accept the default bend radius specified in the active sheet metal style, enter a different value, or click the down arrow to select Measure, Show Dimensions, or List Parameters to enter a different value.
  5. 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. Selected edges must be parallel to create a bend.

    Faces are automatically trimmed or extended to create the bend.

  6. Optionally, click Extend Bend Aligned to Side Faces to extend material along the faces on the side of the edges connected by the bend.
 
  1. 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 one of the following methods for creating a Double Bend between the sheet metal faces:
    • Fix Edges Click to create two equal bends between the faces.

      Depending on the distance between the faces, the bends are tangent or a new face is created between the bends. The faces are not trimmed or extended.

    • 45 Degree Click to create 45 degree bends between selected sheet metal faces.

      Depending on the distance between the faces, the bends are tangent or a new face is created at a 45 degree angle between the bends.

    • Full Radius Click to create a semi-circular bend between selected faces.

      Depending on the size of the selected faces, they are trimmed or extended to create the bend.

    • 90 Degree Click to create 90 degree bends between selected faces.

      Depending on the distance between the faces, the bends are tangent or a new face is created at a 90 degree angle between the bends. Faces are trimmed or extended to create the bends.

  2. 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.
  3. Click OK. Optionally, click Apply to create the face and keep the dialog open to create additional faces.

Override default sheet metal style settings

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.

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.
Parent topic: Face in sheet metal