Face to PlanarSketch

By Adam Nagy

If you want to turn a Face into a PlanarSketch (e.g. in order to get RegionProperties for it) then the following should work.

Create a sketch based on the face, then project all the edges into it. Then you could create a Profile from it, which will of course have RegionProperties:

Sub SketchFromFace()
    ' Before running this code, select the face
    ' you want to create a sketch from
    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument
    
    Dim oFace As Face
    Set oFace = oDoc.SelectSet(1)
    
    Dim oDef As PartComponentDefinition
    Set oDef = oDoc.ComponentDefinition
    
    Dim oSketch As PlanarSketch
    Set oSketch = oDef.Sketches.Add(oFace)
    
    Dim oEdge As Edge
    For Each oEdge In oFace.Edges
        Call oSketch.AddByProjectingEntity(oEdge)
    Next
        
    Dim oProfile As Profile
    Set oProfile = oSketch.Profiles.AddForSolid()
    
    Debug.Print "Area = " + Str(oProfile.RegionProperties.Area)
End Sub

Code in action - just select the face you are interested in:

Additional code for printing RegionProperties data: 
http://adndevblog.typepad.com/manufacturing/2015/09/querying-a-sketch-profile-to-get-regions.html