If you’re using Factory Design Utilities there are some handy tools for including identification tags for components, but if you’re using standard Inventor, you’ll probably be relying on the balloon tools. These allow any property to be included in the balloon (good), but don’t allow much flexibility for auto-positioning the balloons when placing them (for instance central to the component on the drawing view).
In comparison to a product like Revit, which is more focused on large layouts and tagging, there can be quite a lot of manual effort.
What to do?
Well, a training delegate recently made the excellent suggestion of using a model sketch in the part templates for the layout, and then including the sketches in the drawing view. This allows great flexibility with positioning, as the position can be parametrically controlled in the part sketch, and also allows any parameter or iProperty value to be used in the sketch text (for instance).
The only missing link in the chain is how to quickly ‘include’ these sketches in a layout drawing to make them visible. iLogic to the rescue!
Check out the video for an explanation, and see the iLogic code below.
Note: the below video was created by Excitech prior to becoming Symetri in January 2021, following its acquisition by Addnode Group. All Excitech products, services and solutions mentioned in this recording are available through Symetri.
' Start of iLogic code ======================================================================
Sub Main()
Dim Title As String = "Excitech iLogic"
Dim Counter As Integer = 0
Dim SketchName As String = "
Try
Dim oDrawingDoc As DrawingDocument = Nothing
If ThisApplication.ActiveDocument.DocumentType <>
kDrawingDocumentObject Then
MsgBox("This iLogic rule only works with drawing documents!", MsgBoxStyle.OkOnly, Title)
Exit Sub
End If
oDrawingDoc = ThisApplication.ActiveDocument
Dim oView As DrawingView = Nothing
oView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, _
"Select a view to toggle sketch visibility, or hit ESC to cancel...")
If oView Is Nothing Then
Exit Sub
End If
' Get user input for the sketch name
SketchName = InputBox("Please enter name of sketch to toggle visibility.",Title, "Sketch 1")
ThisApplication.UserInterfaceManager.UserInteractionDisabled = True
' Get the referenced document
Dim oDoc As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
If oDoc.DocumentType <> kAssemblyDocumentObject Then
MsgBox("The referenced document needs to be an assembly. Exiting", MsgBoxStyle.OkOnly, Title)
Exit Sub
End If
Dim oAssy As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oOccs As ComponentOccurrences = oAssy.ComponentDefinition.Occurrences
Dim oOcc As ComponentOccurrence = Nothing
Dim TopLevelOcc As ComponentOccurrence = Nothing
Dim Level As Integer = 0
Dim TopLevelAsmDef As AssemblyComponentDefinition = Nothing
Call LoopThroughSubOccurrences(oView, oOccs, oOcc, Level, SketchName, Counter)
Catch
Finally
ThisApplication.UserInterfaceManager.UserInteractionDisabled = False
End Try
ThisApplication.UserInterfaceManager.UserInteractionDisabled = False
If Counter = 0 Then
MsgBox("No sketches called " & SketchName & " were found in this view.", MsgBoxStyle.OkOnly, Title)
End If
End Sub
Sub LoopThroughSubOccurrences(ByRef oDrawView As DrawingView, _
ByRef oOccs As ComponentOccurrences, _
ByRef oOcc As ComponentOccurrence, _
ByRef Level As Integer, _
ByVal SketchName As String, _
ByRef Counter As Integer)
For Each oOcc In oOccs
If oOcc.DefinitionDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
' Get the occurrences in this sub-assembly and loop recursively...
oOccs = oOcc.SubOccurrences
Call LoopThroughSubOccurrences(oDrawView, oOccs, oOcc, Level, SketchName, Counter)
ElseIf oOcc.DefinitionDocumentType = DocumentTypeEnum.kPartDocumentObject Then
' Loop through all sketches
Dim oDef As PartComponentDefinition = oOcc.Definition
Dim oSk As PlanarSketch = Nothing
Dim oSks As PlanarSketches = oDef.Sketches
For Each oSk In oSks
If oSk.Name = SketchName Then
Counter += 1
Dim oSkProx As PlanarSketchProxy = Nothing
Call oOcc.CreateGeometryProxy(oSk, oSkProx)
' Inclusion
Call IncludeSketch(oDrawView, oSkProx)
' Visibility
'Call VisibleSketch(oDrawView, oSkProx)
End If
Next
End If
Next
End Sub
Sub IncludeSketch(ByRef oDrawView As DrawingView, ByVal oSketch As PlanarSketchProxy)
' Toggle inclusion of sketch in drawing view
' Current
Dim Current As Boolean = oDrawView.GetIncludeStatus(oSketch)
oDrawView.SetIncludeStatus(oSketch, Not Current)
End Sub
Sub VisibleSketch(ByRef oDrawView As DrawingView, ByVal oSketch As PlanarSketchProxy)
' Toggle visibility of sketch in drawing view
Dim Current As Boolean = oDrawView.GetVisibility(oSketch)
oDrawView.SetVisibility(oSketch, Not Current)
End Sub
' End of iLogic code ================================================================
