Create and Edit an Extrude Feature with a pocket

Public Sub EditExtrudeFeature()
    ' Create a new part document, using the default part template.
    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.Documents.Add(kPartDocumentObject, _
    ThisApplication.FileManager.GetTemplateFile(kPartDocumentObject))

    ' Set a reference to the component definition.
    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oPartDoc.ComponentDefinition

    ' Create a new sketch on the X-Y work plane.
    Dim oSketch As PlanarSketch
    Set oSketch = oCompDef.Sketches.Add(oCompDef.WorkPlanes(3))

    ' Set a reference to the transient geometry object.
    Dim oTransGeom As TransientGeometry
    Set oTransGeom = ThisApplication.TransientGeometry

    ' Draw a 4cm x 3cm rectangle with the corner at (0,0)
    Dim oRectangleLines As SketchEntitiesEnumerator
    Set oRectangleLines = oSketch.SketchLines.AddAsTwoPointRectangle( _
    oTransGeom.CreatePoint2d(0, 0), _
    oTransGeom.CreatePoint2d(4, 3))

    ' Create a profile.
    Dim oProfile As Profile
    Set oProfile = oSketch.Profiles.AddForSolid

    ' Create a base extrusion 1cm thick.
    Dim oExtrudeDef As ExtrudeDefinition
    Set oExtrudeDef = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kJoinOperation)
    Call oExtrudeDef.SetDistanceExtent(1, kNegativeExtentDirection)
    Dim oExtrude1 As ExtrudeFeature
    Set oExtrude1 = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)

    ' Get the top face of the extrusion to use for creating the new sketch.
    Dim oFrontFace As Face
    Set oFrontFace = oExtrude1.StartFaces.Item(1)

    ' Create a new sketch on this face, but use the method that allows you to
    ' control the orientation and orgin of the new sketch.
    Set oSketch = oCompDef.Sketches.AddWithOrientation(oFrontFace, _
    oCompDef.WorkAxes.Item(1), True, True, oCompDef.WorkPoints(1))

    ' Determine where in sketch space the point (0.5,0.5,0) is.
    Dim oCorner As Point2d
    Set oCorner = oSketch.ModelToSketchSpace(oTransGeom.CreatePoint(0.5, 0.5, 0))

    ' Create the interior 3cm x 2cm rectangle for the pocket.
    Set oRectangleLines = oSketch.SketchLines.AddAsTwoPointRectangle( _
    oCorner, oTransGeom.CreatePoint2d(oCorner.X + 3, oCorner.Y + 2))

    ' Create a profile.
    Set oProfile = oSketch.Profiles.AddForSolid

    ' Create a pocket .25 cm deep (using distance extent).
    Set oExtrudeDef = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kCutOperation)
    Call oExtrudeDef.SetDistanceExtent(0.25, kNegativeExtentDirection)
    Dim oExtrude2 As ExtrudeFeature
    Set oExtrude2 = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)

    ' Move the end of part above this extrude feature since the edit
    ' we are going to perform on this feature involves BREP input.
    Call oExtrude2.SetEndOfPart(True)

    ' Get the back face of the first extrusion to use as termination plane.
    Dim oBackFace As Face
    Set oBackFace = oExtrude1.EndFaces.Item(1)

    ' Change the extent type of the feature.
    Call oExtrude2.Definition.SetToExtent(oBackFace, False)

    ' Move the end of part back to bottom of the feature tree.
    Call oCompDef.SetEndOfPartToTopOrBottom(False)

    ' The following edit of the feature does not involve BREP input.
    ' Hence, no need to move the end of part.
    Call oExtrude2.Definition.SetDistanceExtent(0.25, kNegativeExtentDirection)
End Sub