Sketch Copy Not working: Any transform missing?

[Anonymous]

In Sheet Metal Environment I wish to extract CUT's profile and create a new body by EXTRUDing that profile. But when I copy sketch contents from old to a new one, they appear somewhere else. Why? Am I not looking at certain transforms. 

Here is the code I am trying:

        Private Function CreateNewSketch(faceSketch As PlanarSketch) As PlanarSketch
            CreateNewSketch = Nothing
            Dim pl As WorkPlane = GetWorkPlane(faceSketch.PlanarEntity)

            Dim newsketch As PlanarSketch = Nothing
            Try
                newsketch = m_compDef.Sketches.Add(pl)
                faceSketch.CopyContentsTo(newsketch)
            Catch ex As Exception
                MsgBox(ex.Message)
            End Try
            CreateNewSketch = newsketch
        End Function

And here is the result:

[Jef_E]

My guess is that it looses it's constraint points?

[adam.nagy · Accepted solution]

Hi,

Not sure why you are using "GetWorkPlane". Because of that the new sketch will be based on a different entity and so its origin point will be different. 

If you really need to do that then either move the copied entities based on the origin difference, or you could even set the OriginPoint property of the new skecth so that it will line up with the origin of the original skecth.

E.g. this VBA code works fine - just select the original skecth in the UI first:

Sub CopySketch3()
    Dim faceSketch As PlanarSketch
    Set faceSketch = ThisApplication.ActiveDocument.SelectSet(1)

    Dim pl As Object
    Set pl = faceSketch.PlanarEntity

    Dim compDef As PartComponentDefinition
    Set compDef = ThisApplication.ActiveDocument.ComponentDefinition

    Dim newsketch As PlanarSketch
    Set newsketch = compDef.Sketches.Add(pl)
    Call faceSketch.CopyContentsTo(newsketch)
End Sub

Cheers,

[Anonymous]

Perfect!!! Different Origin must have been the reason. Thanks a lot for precise help.