iLogic turn off visibility of all solids that have "-" in the name in a drawing view

[martin.jerabekM5BZE]

Hi all,

I'm looking for a code, that will work in a drawing view. I need to hide all solids in all parts in the assembly and subassemblies  in that view, that have a "-" in the name (-hole). So it should go through all the parts and all assemblies in that model view and turn off visibility of any solid that have a "-" in the name (or probably easier exact name "-hole").

I did find a code, that kind of works for single part, but I dont know how to make it for assembly and all parts in it. And also the list of solid names is not necessary for me. Here is that code from WCrihfield:

Dim oDDoc As DrawingDocument = ThisDoc.Document
Dim oView As DrawingView = oDDoc.ActiveSheet.DrawingViews.Item(1)
Dim oModel As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
If oModel.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
	Dim oPDoc As PartDocument = oModel
	If oPDoc.ComponentDefinition.HasMultipleSolidBodies = False Then Exit Sub
	Dim oBodies As SurfaceBodies = oPDoc.ComponentDefinition.SurfaceBodies
	Dim oBody3 As SurfaceBody = oBodies.Item(3)
	Dim oBodyGeomInView As DrawingCurvesEnumerator = oView.DrawingCurves(oBody3)
	If oBodyGeomInView.Count = 0 Then Exit Sub
	For Each oDC As DrawingCurve In oBodyGeomInView
		For Each oDCS As DrawingCurveSegment In oDC.Segments
			oDCS.Visible = False
		Next
	Next
End If

Thank you all

[Andrii_Humeniuk]

Hi @martin.jerabekM5BZE . The code looks for the character "-" in the body name (line 24).

Sub main
	Dim oInvApp As Inventor.Application = ThisApplication
	Dim oDDoc As DrawingDocument = oInvApp.ActiveDocument
	Dim oTM As TransactionManager = oInvApp.TransactionManager
	Dim newTM As Transaction = oTM.StartTransaction(oDDoc, "ChangeCurvesColor")
	For Each oSheet As Sheet In oDDoc.Sheets
		For Each oView As DrawingView In oSheet.DrawingViews
			If oView.ViewStyle = DrawingViewStyleEnum.kShadedDrawingViewStyle Then Continue For
			Dim oRefDoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
			Dim oRefDef As AssemblyComponentDefinition = oRefDoc.ComponentDefinition
			Call ChangeCutCurvesView(oView, oRefDef.Occurrences)
		Next
	Next
	newTM.End()
End Sub

Private Function ChangeCutCurvesView(ByVal oView As DrawingView, ByVal oOccs As ComponentOccurrences)
	For Each oOcc As ComponentOccurrence In oOccs
		If TypeOf oOcc.Definition Is PartComponentDefinition Or _
			TypeOf oOcc.Definition Is SheetMetalComponentDefinition Then
			Dim oCompDef As ComponentDefinition = oOcc.Definition
			If oOcc.SurfaceBodies.Count > 1 Then
				For Each oBody As SurfaceBody In oOcc.SurfaceBodies
					If oBody.Name.Contains("-") Then
						oCurves = oView.DrawingCurves(oBody)
						For Each oCurve As DrawingCurve In oCurves	
							For Each oSegment As DrawingCurveSegment In oCurve.Segments
								oSegment.Visible = False
							Next
						Next
					End If
				Next
			End If
		End If
		If oOcc.SubOccurrences IsNot Nothing Then
			Call ChangeCutCurvesView(oView, oOcc.SubOccurrences)
		End If
	Next
End Function

[martin.jerabekM5BZE]

Hello Andrii_Humeniuk,

thank you for the code. But I'm having an error message when I'm trying to run it. Does it work for you? How do you proceed? (slelect view and run the rule? I have Inventor 2023 latest update.

Thank you

[Andrii_Humeniuk]

In my case the code works fine. I added an "On Error Resume Next" statement (line 27), if that doesn't help you, you'll have to catch the error to figure out what the problem is.

Sub main
	Dim oInvApp As Inventor.Application = ThisApplication
	Dim oDDoc As DrawingDocument = oInvApp.ActiveDocument
	Dim oTM As TransactionManager = oInvApp.TransactionManager
	Dim newTM As Transaction = oTM.StartTransaction(oDDoc, "ChangeCurvesColor")
	For Each oSheet As Sheet In oDDoc.Sheets
		For Each oView As DrawingView In oSheet.DrawingViews
			If oView.ViewStyle = DrawingViewStyleEnum.kShadedDrawingViewStyle Then Continue For
			Dim oRefDoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
			Dim oRefDef As AssemblyComponentDefinition = oRefDoc.ComponentDefinition
			Call ChangeCutCurvesView(oView, oRefDef.Occurrences)
		Next
	Next
	newTM.End()
End Sub

Private Function ChangeCutCurvesView(ByVal oView As DrawingView, ByVal oOccs As ComponentOccurrences)
	For Each oOcc As ComponentOccurrence In oOccs
		If TypeOf oOcc.Definition Is PartComponentDefinition Or _
			TypeOf oOcc.Definition Is SheetMetalComponentDefinition Then
			Dim oCompDef As ComponentDefinition = oOcc.Definition
			If oOcc.SurfaceBodies.Count > 1 Then
				For Each oBody As SurfaceBody In oOcc.SurfaceBodies
					If oBody.Name.Contains("-") Then
						oCurves = oView.DrawingCurves(oBody)
						For Each oCurve As DrawingCurve In oCurves	
							On Error Resume Next
							For Each oSegment As DrawingCurveSegment In oCurve.Segments
								oSegment.Visible = False
							Next
						Next
					End If
				Next
			End If
		End If
		If oOcc.SubOccurrences IsNot Nothing Then
			Call ChangeCutCurvesView(oView, oOcc.SubOccurrences)
		End If
	Next
End Function

[martin.jerabekM5BZE]

OK I did a test and it works for normal parts. But it does not hide lines in an ISO view. Why it doesn't work for ISO?

And that error I'm having is related to iParts. Lots of my parts are an iParts. Can that code be adapted to do all, normal parts and iParts?

So this code works actually with hiding the lines of those solids. Wouldn't be a code with changing visibility of those solids in that view easier?

Thank you

[martin.jerabekM5BZE]

OK, I removed that part of code with specification of view style, as it is not requested and it should work for all types. But the problem with iPart solids stays.

Code:

Sub main
	Dim oInvApp As Inventor.Application = ThisApplication
	Dim oDDoc As DrawingDocument = oInvApp.ActiveDocument
	Dim oTM As TransactionManager = oInvApp.TransactionManager
	Dim newTM As Transaction = oTM.StartTransaction(oDDoc, "ChangeCurvesColor")
	For Each oSheet As Sheet In oDDoc.Sheets
		For Each oView As DrawingView In oSheet.DrawingViews
			Dim oRefDoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
			Dim oRefDef As AssemblyComponentDefinition = oRefDoc.ComponentDefinition
			Call ChangeCutCurvesView(oView, oRefDef.Occurrences)
		Next
	Next
	newTM.End()
End Sub

Private Function ChangeCutCurvesView(ByVal oView As DrawingView, ByVal oOccs As ComponentOccurrences)
	For Each oOcc As ComponentOccurrence In oOccs
		If TypeOf oOcc.Definition Is PartComponentDefinition Or _
			TypeOf oOcc.Definition Is SheetMetalComponentDefinition Then
			Dim oCompDef As ComponentDefinition = oOcc.Definition
			If oOcc.SurfaceBodies.Count > 1 Then
				For Each oBody As SurfaceBody In oOcc.SurfaceBodies
					If oBody.Name.Contains("-") Then
						oCurves = oView.DrawingCurves(oBody)
						For Each oCurve As DrawingCurve In oCurves	
							On Error Resume Next
							For Each oSegment As DrawingCurveSegment In oCurve.Segments
								oSegment.Visible = False
							Next
						Next
					End If
				Next
			End If
		End If
		If oOcc.SubOccurrences IsNot Nothing Then
			Call ChangeCutCurvesView(oView, oOcc.SubOccurrences)
		End If
	Next
End Function

Still I'd rather change visibility of actual solids, as hiding lines sometimes makes areas without lines on an ISO views.

Thank you very much for your help

[Andrii_Humeniuk]

Try this code:

Sub main
	Dim oInvApp As Inventor.Application = ThisApplication
	Dim oDDoc As DrawingDocument = oInvApp.ActiveDocument
	Dim oTM As TransactionManager = oInvApp.TransactionManager
	Dim newTM As Transaction = oTM.StartTransaction(oDDoc, "ChangeCurvesColor")
	For Each oSheet As Sheet In oDDoc.Sheets
		For Each oView As DrawingView In oSheet.DrawingViews
			Dim oRefDoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
			Dim oRefDef As AssemblyComponentDefinition = oRefDoc.ComponentDefinition
			Call ChangeCutCurvesView(oView, oRefDef.Occurrences)
		Next
	Next
	newTM.End()
End Sub

Private Function ChangeCutCurvesView(ByVal oView As DrawingView, ByVal oOccs As ComponentOccurrences)
	For Each oOcc As ComponentOccurrence In oOccs
		If TypeOf oOcc.Definition Is PartComponentDefinition Or _
			TypeOf oOcc.Definition Is SheetMetalComponentDefinition Then
			Dim oCompDef As ComponentDefinition = oOcc.Definition
			If oOcc.SurfaceBodies.Count > 1 Then
				For Each oBody As SurfaceBody In oOcc.SurfaceBodies
					If oBody.Name.Contains("-") Then
						oView.SetVisibility(oBody, False)
					End If
				Next
			End If
		End If
		If oOcc.SubOccurrences IsNot Nothing Then
			Call ChangeCutCurvesView(oView, oOcc.SubOccurrences)
		End If
	Next
End Function

[martin.jerabekM5BZE]

Thank you,

nice, that works almost flawlessly. I have an assembly with suppressed parts and that obviously causes an error as I tried to run that code with an assembly without suppressed parts and there it works great. Can you add to that code a line, were it will not go through suppressed parts? That could hopefully help.

Is there any possibility to dhave 2 cases of running?

1. Not selected a view - so it goes through all views on the list

2. Selected a single view - it hides just solids on that selected view

Thank you, you are genius

[Andrii_Humeniuk · Accepted solution]

No problem... Try this code:

Sub main
	Dim oInvApp As Inventor.Application = ThisApplication
	Dim oDDoc As DrawingDocument = oInvApp.ActiveDocument
	Dim oTM As TransactionManager = oInvApp.TransactionManager
	Dim vbResult As DialogResult = MessageBox.Show("Choose a separate view?", _
												   "Chooseview", _
												   MessageBoxButtons.YesNoCancel, _
												   MessageBoxIcon.Question, _
												   MessageBoxDefaultButton.Button1)
	If vbResult = vbCancel Then Exit Sub
	Dim newTM As Transaction = oTM.StartTransaction(oDDoc, "ChangeCurvesColor")
	If vbResult = vbYes Then
		Dim oView As DrawingView
		oView = oInvApp.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select view...")
		If oView Is Nothing Then Exit Sub
		Dim oRefDoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
		Dim oRefDef As AssemblyComponentDefinition = oRefDoc.ComponentDefinition
		Call ChangeCutCurvesView(oView, oRefDef.Occurrences)
	Else
		For Each oSheet As Sheet In oDDoc.Sheets
			For Each oView As DrawingView In oSheet.DrawingViews
				Dim oRefDoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
				Dim oRefDef As AssemblyComponentDefinition = oRefDoc.ComponentDefinition
				Call ChangeCutCurvesView(oView, oRefDef.Occurrences)
			Next
		Next
	End If
	newTM.End()
End Sub

Private Function ChangeCutCurvesView(ByVal oView As DrawingView, ByVal oOccs As ComponentOccurrences)
	For Each oOcc As ComponentOccurrence In oOccs
		If oOcc.Suppressed Then Continue For
		If TypeOf oOcc.Definition Is PartComponentDefinition Or _
			TypeOf oOcc.Definition Is SheetMetalComponentDefinition Then
			Dim oCompDef As ComponentDefinition = oOcc.Definition
			If oOcc.SurfaceBodies.Count > 1 Then
				For Each oBody As SurfaceBody In oOcc.SurfaceBodies
					If oBody.Name.Contains("-") Then
						oView.SetVisibility(oBody, False)
					End If
				Next
			End If
		End If
		If oOcc.SubOccurrences IsNot Nothing Then
			Call ChangeCutCurvesView(oView, oOcc.SubOccurrences)
		End If
	Next
End Function

[martin.jerabekM5BZE]

Awesome!! One more thing as a safety. When the Design view is not set to Primary but another and set to Associative, a bug error appears. Can be in the code written, that it check if the Design view is associative and if yes, then cancels this associativity first and continue?

Thank you very much for your help.

[martin.jerabekM5BZE · Accepted solution]

Final code is here: It changes Design View to not Associative before it hides those solids. If the view was Associative, it produced error.

Sub main
	Dim oInvApp As Inventor.Application = ThisApplication
	Dim oDDoc As DrawingDocument = oInvApp.ActiveDocument
	Dim oTM As TransactionManager = oInvApp.TransactionManager
	Dim vbResult As DialogResult = MessageBox.Show("Choose a separate view?", _
												   "Chooseview", _
												   MessageBoxButtons.YesNoCancel, _
												   MessageBoxIcon.Question, _
												   MessageBoxDefaultButton.Button1)
	If vbResult = vbCancel Then Exit Sub
	Dim newTM As Transaction = oTM.StartTransaction(oDDoc, "ChangeCurvesColor")
	If vbResult = vbYes Then
		Dim oView As DrawingView
		oView = oInvApp.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select view...")
		If oView Is Nothing Then Exit Sub
		Dim oRefDoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
		Dim oRefDef As AssemblyComponentDefinition = oRefDoc.ComponentDefinition
		
		If oView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
                Dim name As String: name = oView.DesignViewRepresentation
                Call oView.SetDesignViewRepresentation(name, False)
        End If
		
		Call ChangeCutCurvesView(oView, oRefDef.Occurrences)
	Else
		For Each oSheet As Sheet In oDDoc.Sheets
			For Each oView As DrawingView In oSheet.DrawingViews
				Dim oRefDoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
				Dim oRefDef As AssemblyComponentDefinition = oRefDoc.ComponentDefinition
				
		If oView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
                Dim name As String: name = oView.DesignViewRepresentation
                Call oView.SetDesignViewRepresentation(name, False)
        End If
				
				Call ChangeCutCurvesView(oView, oRefDef.Occurrences)
			Next
		Next
	End If
	newTM.End()
End Sub

Private Function ChangeCutCurvesView(ByVal oView As DrawingView, ByVal oOccs As ComponentOccurrences)
	For Each oOcc As ComponentOccurrence In oOccs
		If oOcc.Suppressed Then Continue For
		If TypeOf oOcc.Definition Is PartComponentDefinition Or _
			TypeOf oOcc.Definition Is SheetMetalComponentDefinition Then
			Dim oCompDef As ComponentDefinition = oOcc.Definition
			If oOcc.SurfaceBodies.Count > 1 Then
				For Each oBody As SurfaceBody In oOcc.SurfaceBodies
					If oBody.Name.Contains("-") Then
						oView.SetVisibility(oBody, False)
					End If
				Next
			End If
		End If
		If oOcc.SubOccurrences IsNot Nothing Then
			Call ChangeCutCurvesView(oView, oOcc.SubOccurrences)
		End If
	Next
End Function

[martin.jerabekM5BZE]

Hi, how dificult is to add to the code, that it works also for views from ipn (presentation) files? Thank you