Read the instance property in the occurrences of a drawing

[kv5053545]

I do not know if you can help me I have an assembly with many occurrences when I want to dimension them in an automatic way it has been complicating me a lot, I just found out that there are the instance property I do not know if it is possible to read them from the code so that if it finds a certain letter in the instance property inside the occurrence it makes the dimensions.

Dim drawingDoc As DrawingDocument = ThisApplication.ActiveDocument

' Loop through each sheet in the drawing document
For Each sheet As Sheet In drawingDoc.Sheets
    ' Loop through each view on the sheet
    For Each view As DrawingView In Sheet.DrawingViews
        If View.Name = "VIEW1" Then
            ' Check if the view is an assembly view
            ' Get the assembly document for the view
            Dim asmDoc As AssemblyDocument = View.ReferencedDocumentDescriptor.ReferencedDocument

            ' Loop through each assembly component
 For Each comp As ComponentOccurrence In asmDoc.ComponentDefinition.Occurrences
                Dim componentName As String = comp.Name
                Dim Search As String = "Wall"

                If componentName.Contains(Search) Then
 ' Add a dimension to the component if the component name contains "Wall"
Dim ShGeneral = ThisDrawing.Sheets.ItemByName("General:1") 
Dim genDims = ShGeneral.DrawingDimensions.GeneralDimensions
Dim view1 = ShGeneral.DrawingViews.ItemByName("VIEW1") 
 Dim wPl_Wall_FlangeLeft  = view1.GetIntent(comp.Name, "WPl_Wall-FlangeLeft")
 Dim wPl_Wall_FlangeRight = view1.GetIntent(comp.Name, "WPl_Wall-FlangeRight")
  Dim dimX As Double 
 Dim dimY As Double
           '' Add the dimension to the drawing
  Dim linDim1 = genDims.AddLinear("Width_" & componente, view1.SheetPoint(dimX, dimY), wPl_Wall_FlangeLeft, wPl_Wall_FlangeRight)
                        End If

            Next
        End If
    Next
Next

[dalton98 · Accepted solution]

Yes this is doable. Instance properties are unique for the assembly they are in. They are separate from the typical property sets in an inventor file.

https://modthemachine.typepad.com/my_weblog/2010/02/accessing-iproperties.html

Here is an example of how to access them:

Dim oADoc As AssemblyDocument = ThisDoc.Document
For Each comp As ComponentOccurrence In oADoc.ComponentDefinition.Occurrences

	'check if instance property exists
	If comp.OccurrencePropertySetsEnabled = True
		Dim instanceSearch As String = "test"
		For i = 1 To comp.OccurrencePropertySets(1).Count
'			If comp.OccurrencePropertySets(1)(i).Name.Contains("test")
				MessageBox.Show(comp.OccurrencePropertySets(1)(i).Name, comp.OccurrencePropertySets(1)(i).Value)
'			End If
		Next
	End If
Next

[kv5053545]

Hi, @dalton98  I have seen how to access to the instance property of the occurrences of an assembly but when I try to do the same inside the occurrences that are inside a view in a drawing, I get this error: iProperties: The component named "Wall_A:1" was not found.

Dim drawingDoc As DrawingDocument = ThisApplication.ActiveDocument

' Loop through each sheet in the drawing document
For Each sheet As Sheet In drawingDoc.Sheets
    ' Loop through each view on the sheet
    For Each view As DrawingView In Sheet.DrawingViews
        If View.Name = "VIEW1" Then
            ' Check if the view is an assembly view
            ' Get the assembly document for the view
            Dim asmDoc As AssemblyDocument = View.ReferencedDocumentDescriptor.ReferencedDocument

            ' Loop through each assembly component
            For Each comp As ComponentOccurrence In asmDoc.ComponentDefinition.Occurrences
                Dim componente As String = comp.Name 
				
                Dim searchWalls As String = "Wall"

                If componente.Contains(searchWalls) Then
                    ' Add a dimension to the component if the component name contains "Wall"
                    Dim ShGeneral = ThisDrawing.Sheets.ItemByName("General:1") 
                    Dim genDims = ShGeneral.DrawingDimensions.GeneralDimensions
                    Dim view1 = ShGeneral.DrawingViews.ItemByName("VIEW1") 
                    Dim wPl_Wall_FlangeLeft  = view1.GetIntent(componente, "WPl_Wall-FlangeLeft")
                    Dim wPl_Wall_FlangeRight = view1.GetIntent(componente, "WPl_Wall-FlangeRight")
					  
					   
					Dim side = iProperties.InstanceValue(componente, "Side")

                    Dim dimX As Double = 0
                    Dim dimY As Double = 0

If side = A Then
	
	   Dim linDim1 = genDims.AddLinear("SideA" & componente, view1.SheetPoint(dimX, dimY), wPl_Wall_FlangeLeft, wPl_Wall_FlangeRight)
Else If side = B
	
	   Dim linDim1 = genDims.AddLinear("SideB" & componente, view1.SheetPoint(dimX, dimY), wPl_Wall_FlangeLeft, wPl_Wall_FlangeRight)
ElseIf side = C
	
	   Dim linDim1 = genDims.AddLinear("SideC" & componente, view1.SheetPoint(dimX, dimY), wPl_Wall_FlangeLeft, wPl_Wall_FlangeRight)
Else If side = D
	
   Dim linDim1 = genDims.AddLinear("SideD" & componente, view1.SheetPoint(dimX, dimY), wPl_Wall_FlangeLeft, wPl_Wall_FlangeRight)
End If
                  
                End If
            Next
        End If
    Next
Next

		

[A.Acheson]

Hi @kv5053545 

Try using the occurrence name to target the correct document

Dim side = iProperties.InstanceValue(componente.Name, "Side")

If that doesn't work then you can try the longer API method that Dalton referred too.

'check if instance property exists
	If componente.OccurrencePropertySetsEnabled = True
		Dim instanceSearch As String = "Side"
		For i = 1 To componente.OccurrencePropertySets(1).Count
			If componente.OccurrencePropertySets(1)(i).Name.Contains(instanceSearch)
				MessageBox.Show(componente.OccurrencePropertySets(1)(i).Name, componente.OccurrencePropertySets(1)(i).Value)
			End If
		Next
	End If

[kv5053545]

Hi  @A.Acheson @dalton98 ,  Thank you very much, I was able to implement it in my code and it worked very well.
Do you know if it is now possible to create instance property from vb.net to inventor?

[dalton98]

edit* do it this way

Dim oADoc As AssemblyDocument = ThisDoc.Document
Dim comp As ComponentOccurrence = oADoc.ComponentDefinition.Occurrences(1)

iProperties.InstanceValue(comp.Name, "test") = "hello"

@kv5053545 You would add instance values the same way as you find them

Enable property sets for the occurrence > add instance property in the first property set

Dim oADoc As AssemblyDocument = ThisDoc.Document
Dim comp As ComponentOccurrence = oADoc.ComponentDefinition.Occurrences(1)
comp.OccurrencePropertySetsEnabled = True
Dim instProp As Inventor.Property = comp.OccurrencePropertySets(1).Add(12, "name")