Turn off model sketches in drawing

[Cadkunde.nl]

Hello everyone, I got the following problem:

I have a drawing with 1 view of a part.

I get the model sketches of that part in a drawing view

If you right click that sketch you can choose "Include" and "Visible"

Now I made the following code in ilogic:

Sub Main()
    Dim oDoc As DrawingDocument = ThisDoc.Document
    Dim oSheet As Sheet = oDoc.ActiveSheet
    Dim oNode As BrowserNode = oDoc.BrowserPanes("Model").GetBrowserNodeFromObject(oSheet.DrawingViews.Item(1))

    Call recurseNodes(oNode)
End Sub

Sub recurseNodes(node As BrowserNode)
     
    Dim bn As BrowserNode
    
    For Each bn In node.BrowserNodes

            If TypeName(bn.NativeObject) = "PlanarSketch" Then
                bn.Visible = False
                MsgBox(bn.Visible)
                Dim oSketch As PlanarSketch = bn.NativeObject
                oSketch.Visible = False
                MsgBox(oSketch.Visible)
                Dim oProxy As PlanarSketchProxy = TryCast(oSketch, PlanarSketchProxy)

                If oProxy Is Nothing Then MsgBox("fail")

            End If
            If Not TypeName(bn.NativeObject) = "DrawingView" Then
                Call recurseNodes(bn)
            Else
                Continue For
            End If
    Next
End Sub

Now the messageboxes say that sketches are turned off,  but in truth nothing happens, sketches remain on.

What am I doing wrong?

Thanks in advance,

Arnold

[MechMachineMan]

Try this. If it doesn't work, try uncommenting the lines and trying it with the command I have in there.

Sub Main()
    Dim oDoc As DrawingDocument = ThisDoc.Document
    Dim oSheet As Sheet = oDoc.ActiveSheet
    Dim oNode As BrowserNode = oDoc.BrowserPanes("Model").GetBrowserNodeFromObject(oSheet.DrawingViews.Item(1))

    Call recurseNodes(oNode)
End Sub

Sub recurseNodes(node As BrowserNode)
     
    Dim bn As BrowserNode
    'Dim oCommandMgr As CommandManager
    'oCommandMgr = ThisApplication.CommandManager
    'Dim oControlDef1 As ControlDefinition
    For Each bn In node.BrowserNodes

            If TypeName(bn.NativeObject) = "PlanarSketch" Then
                bn.EnsureVisible = true
                bn.Visible = True
                'bn.DoSelect
                'oControlDef1 = oCommandMgr.ControlDefinitions.Item("DrawingEntityVisibilityCtxCmd")
            'oControlDef1.Execute
                    
                Dim oSketch As PlanarSketch = bn.NativeObject
                oSketch.Visible = False

              
                MsgBox(oSketch.Visible)
                Dim oProxy As PlanarSketchProxy = TryCast(oSketch, PlanarSketchProxy)

                If oProxy Is Nothing Then MsgBox("fail")

            End If
            If Not TypeName(bn.NativeObject) = "DrawingView" Then
                Call recurseNodes(bn)
            Else
                Continue For
            End If
    Next
End Sub

[MechMachineMan]

Looking a little deeper,

http://help.autodesk.com/view/INVNTOR/2018/ENU/?guid=GUID-D273D9C3-C24F-4CDD-B571-F2C0B5F7A5B3

reveals that .SetIncludeStatus and .SetVisibility are likely much better bets.

[Cadkunde.nl]

Yes, I got it working now. Thanks

Dim oProxy As PlanarSketchProxy = TryCast(oSketch, PlanarSketchProxy)
 oDoc.Sheets(1).DrawingViews(1).SetVisibility(oSketch, False)

When I did bn.visible it actually turned the sketch of in the part

I tried bn.BrowserNodeDefinition.Visible but that completely removed the node from the browser

I was fooled that the Include and Visibility were properties of the browsernode rather than the drawingview.