Trying to use AddByProjectingEntity with a DrawingSketch

[larry.daubenspeck]

Help!  I am trying to project geometry (a floor plan) onto a DrawingSketch using the AddByProjectingEntity method.  The active document is a Drawing; I have created the DrawingSketch from the active view.  Yet nothing I try seems to work.  Can it really be that difficult?  A sample of one of my attempts follows.  What am I missing?

'Get the drawing document.        

Dim thisDwg As DrawingDocument = InvApp.ActiveDocument

'Get the sheet.        

Dim thisSheet As Sheet = thisDwg.ActiveSheet

'Get the active view.        

Dim thisView As DrawingView = thisSheet.DrawingViews.Item(1)

'Create a sketch.        

Dim thisDwgSketch As DrawingSketch = thisView.Sketches.Add

'Start editing the sketch.        

thisDwgSketch.Edit()

'Get the referenced assembly document.        

Dim AssyDoc As AssemblyDocument = thisView.ReferencedDocumentDescriptor.ReferencedDocument        

Dim AssyCompDef As AssemblyComponentDefinition = AssyDoc.ComponentDefinition        

Dim Backstop1 As ComponentOccurrence = AssyCompDef.Occurrences.Item(1)

Dim Gym1 As ComponentOccurrence = Nothing        

For Each Gym1 In Backstop1.Definition.Occurrences            

     If InStr(Gym1.Name, "GYM") Then                

          Exit For            

     End If        

Next

Dim oOccur As ComponentOccurrence = Nothing        

For Each oOccur In Gym1.Definition.Occurrences            

     If InStr(oOccur.Name, "WALLS") Then                

          For Each SurfBody As SurfaceBody In oOccur.SurfaceBodies                    

               For Each oEdge As Edge In SurfBody.Edges                        

                    Dim anObject As Object = Nothing                        

                    oOccur.CreateGeometryProxy(oEdge, anObject)                        

                    thisDwgSketch.AddByProjectingEntity(anObject)                    

               Next                

          Next                

          Exit For            

     End If        

Next

thisDwgSketch.ExitEdit()

[ekinsb]

When using the AddByProjectingEntity method in a drawing you need to provide an entity that exists in the context of a drawing.  You were getting the edge in the context of the assembly.  The object that represents an edge in the drawing is a DrawingCurve object.  I converted your program to VBA because it's quicker to test and modified it to work.  In my test I had a simple assembly with two parts where one of them is named "BoxInPocket".  It looks for this part and then projects all of its edges onto the newly created sketch. 

Public Sub ProjectEntity()
    'Get the drawing document.
    Dim thisDwg As DrawingDocument
    Set thisDwg = ThisApplication.ActiveDocument

    'Get the sheet.
    Dim thisSheet As Sheet
    Set thisSheet = thisDwg.ActiveSheet

    'Get the active view.
    Dim thisView As DrawingView
    Set thisView = ThisApplication.CommandManager.Pick(kDrawingViewFilter, _
                                                    "Select the drawing view.")

    'Create a sketch on the view.
    Dim thisDwgSketch As DrawingSketch
    Set thisDwgSketch = thisView.Sketches.Add

    ' Get the referenced assembly.
    Dim asmDoc As AssemblyDocument
    Set asmDoc = thisView.ReferencedDocumentDescriptor.ReferencedDocument
    
    ' Get the occurrence named "BoxInPocket"
    Dim boxOcc As ComponentOccurrence
    For Each boxOcc In asmDoc.ComponentDefinition.Occurrences
        If InStr(boxOcc.Name, "BoxInPocket") Then
            ' Iterate over the the edges in the part.
            ' Since the surface body is obtained from the occurence
            ' it is a SurfaceBodyProxy and will return proxy edges
            ' in the context of the top-level assembly.
            Dim partEdge As Edge
            For Each partEdge In boxOcc.SurfaceBodies.Item(1).Edges
                ' Attempt to get any drawing curves associated with this edge.
                ' This will return curves if the edge is visible in the view.
                Dim drawCurves As DrawingCurvesEnumerator
                Set drawCurves = thisView.DrawingCurves(partEdge)
                
                ' Project each drawing curve onto the sketch.
                Dim drawCurve As DrawingCurve
                For Each drawCurve In drawCurves
                    Dim ent As SketchEntity
                    Set ent = thisDwgSketch.AddByProjectingEntity(drawCurve)
                Next
            Next
        End If
    Next
End Sub

[larry.daubenspeck]

Thanks Brian,

I got your version to work fine, both in VBA and Vb.net.  Mine, however, is still telling me that my parameter is incorrect when it gets to this line:

     Dim drawCurves As DrawingCurvesEnumerator = thisView.DrawingCurves(oEdge)

The only difference that I can tell is that the part I'm wanting to project is a few levels deep into the assembly, whereas yours is a top-level part.  Could that be making a difference?

[xiaodong_liang · Accepted solution]

Hi Larry,

yes, you will have to recurse the sub assembly to get the part. The following code is for you reference.

Public Sub ProjectEntity()
    'Get the drawing document.
    Dim thisDwg As DrawingDocument
    Set thisDwg = ThisApplication.ActiveDocument

    'Get the sheet.
    Dim thisSheet As Sheet
    Set thisSheet = thisDwg.ActiveSheet

    'Get the active view.
    Dim thisView As DrawingView
    Set thisView = ThisApplication.CommandManager.Pick(kDrawingViewFilter, _
                                                    "Select the drawing view.")

    'Create a sketch on the view.
    Dim thisDwgSketch As DrawingSketch
    Set thisDwgSketch = thisView.Sketches.Add

    ' Get the referenced assembly.
    Dim asmDoc As AssemblyDocument
    Set asmDoc = thisView.ReferencedDocumentDescriptor.ReferencedDocument
    
    ' Get the occurrence named "BoxInPocket"
    Dim boxOcc As ComponentOccurrence
    For Each boxOcc In asmDoc.ComponentDefinition.Occurrences
    'For Each boxOcc In asmDoc.ComponentDefinition.Occurrences
        If InStr(boxOcc.Name, "Assembly1:1") Then
            ' Iterate over the the edges in the part.
            ' Since the surface body is obtained from the occurence
            ' it is a SurfaceBodyProxy and will return proxy edges
            ' in the context of the top-level assembly.
            
            '
             Call recurse_occ(boxOcc, thisView, thisDwgSketch)
        End If
    Next
End Sub



Sub recurse_occ(oParentOcc As ComponentOccurrence, thisView As DrawingView, thisDwgSketch As DrawingSketch)

    If TypeOf oParentOcc.Definition Is PartComponentDefinition Then
                Dim partEdge As Edge
                For Each partEdge In oParentOcc.SurfaceBodies.Item(1).Edges
                    ' Attempt to get any drawing curves associated with this edge.
                    ' This will return curves if the edge is visible in the view.
                    Dim drawCurves As DrawingCurvesEnumerator
                    Set drawCurves = thisView.DrawingCurves(partEdge)
                    
                    ' Project each drawing curve onto the sketch.
                    Dim drawCurve As DrawingCurve
                    For Each drawCurve In drawCurves
                        Dim ent As SketchEntity
                        Set ent = thisDwgSketch.AddByProjectingEntity(drawCurve)
                    Next
                Next
             Else
               ' if this occurrence is a sub assembly
                Dim oSubOcc As ComponentOccurrence
                
                For Each oSubOcc In oParentOcc.SubOccurrences
                    Call recurse_occ(oSubOcc, thisView, thisDwgSketch)
                Next
                 
            End If
End Sub

You can also get all referenced documents of the top assembly by AllReferencedDocuments, check which are part, and add the project sketch (similar code above) for them in the drawing.

[larry.daubenspeck]

Thanks Xiaodong,

I finally got it to work, but not as I expected. 

Initially, I searched through the top level assembly to find a particular backstop, and then searched through the backstop to find its gym, and then searched through the gym to find the walls.  This, however, was resulting in an "incorrect parameter" error.

I then modified your method to recursively search, starting at the top, and continue through everything until I arrived at a part with the name I was looking for.  Doing it this way worked.  Not sure why, but at least I can continue on now.

Thanks again.