Automatic addition of dimensions in the drawing

[doma-zieman]

In the assembly drawing.
In the components (parts) the planes are described. 
I want the rule to create a dimension between these planes.
Error displays all the time.


Sub Main()
'[
Dim oDoc As DrawingDocument
oDoc = ThisApplication.ActiveDocument
Dim oSheets As Sheets
oSheets = oDoc.Sheets
Dim oSheet As Sheet
oSheets.Item(1).Activate
oSheet = oDoc.ActiveSheet

Dim nazwa As String = ThisDoc.FileName(False) 'without extension
ZN = Len(nazwa)
znn = ZN - 4
pref = Left(nazwa, ZN - 4)
Dim oView1 As DrawingView
oView1 = oSheet.DrawingViews.Item(1)



'    'Readys code for Creation of reference points for dimension placement
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry


Dim oPt1 As Point2d

oPt1 = oTG.CreatePoint2d(oView1.Left + (oView1.Width / 3), oView1.Top - oView1.Height - 1)


' setting the component name
Dim C0 As String
C0 = pref & "-004:1"
Dim C1 As String
C1 = pref & "-005:2"
Dim C2 As String
C2 = pref & "-005:3"


Dim viewModelDoc = ActiveSheet.View("WIDOK10").ModelDocument

For Each oOcc00 As ComponentOccurrence In viewModelDoc.ComponentDefinition.Occurrences
	If oOcc00.Name = C0 Then
		For Each oOcc1 As ComponentOccurrence In viewModelDoc.ComponentDefinition.Occurrences
			'MessageBox.Show(oOcc00.Name, "Title")
			If oOcc1.Name = C1 Then
				'MessageBox.Show("Title", "Title")
				'MessageBox.Show("C1", "Title")
				PlaceDIMinPart(oView1, oSheet, "Wym2", "WymN", oPt1, oOcc00, oOcc1)
				Exit For
			End If
		Next
		Exit For
	End If
Next

	']  
	End Sub


	Private Function PlaceDIMinPart(oView As DrawingView, oSheet As Sheet, SFaceName As String, EFaceName As String, InsertPT As Point2d, oComp1 As ComponentOccurrence, oComp2 As ComponentOccurrence)
	'[

	Dim aoFace1 As Inventor.FaceProxy
	aoFace1 = FindFace(oView, oSheet, SFaceName, oComp2)

	Dim aoFace2 As Inventor.FaceProxy
	aoFace2 = FindFace(oView, oSheet, EFaceName, oComp1)

	Dim oDrawCurves1 As Inventor.DrawingCurvesEnumerator
	oDrawCurves1 = oView.DrawingCurves(aoFace1)

	Dim aoFace2Edge1 As DrawingCurve
	aoFace2Edge1 = oDrawCurves1.Item(1)

	oDrawCurves2 = oView.DrawingCurves(aoFace2)
	Dim aoFace2Edge2 As DrawingCurve
	aoFace2Edge2 = oDrawCurves2.Item(1)
'[
Dim startPoint2 As Point2d
Dim endPoint2 As Point2d

startPoint2 = aoFace2Edge2.StartPoint
endPoint2 = aoFace2Edge2.EndPoint

Dim startPoint1 As Point2d
Dim endPoint1 As Point2d

startPoint1 = aoFace2Edge1.StartPoint
endPoint1 = aoFace2Edge1.EndPoint
']
'[	'Readys code for creation of general dimensions
	Dim oGeneralDims As GeneralDimensions
	oGeneralDims = oSheet.DrawingDimensions.GeneralDimensions
']

	Dim oDim2 As GeneralDimension
	oDim2 = oGeneralDims.AddLinear(InsertPT, endPoint1 , endPoint2 , kHorizontalDimensionType)
	oDim2.Precision = 0
	Dim oDim2Att As AttributeSet
	oDim2Att = oDim2.AttributeSets.Add("auto")
	']
	End Function

	Function FindFace(oView As DrawingView, oSheet As Sheet, FaceName As String, oComp As ComponentOccurrence) As Inventor.FaceProxy
	'[
	Dim oAssemblyDoc As AssemblyDocument
	oAssemblyDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument
	Dim oTG As TransientGeometry
	oTG = ThisApplication.TransientGeometry
 	Dim oPartDoc As PartDocument = oComp.Definition.Document
	 Dim oObjs As ObjectCollection
    oObjs = oPartDoc.AttributeManager.FindObjects("iLogicEntityNameSet", "iLogicEntityName", FaceName)

	If oObjs.Count > 0 Then
		Dim oFace As Inventor.Face
		oFace = oObjs.Item(1)
		Dim oFaceProxy As Inventor.FaceProxy
		Call oComp.CreateGeometryProxy(oFace, oFaceProxy)
		FindFace = oFaceProxy	
	End If

	']
	End Function


Error in underlined line:
EN:
The COM model object of type 'System.__ComObject' cannot be cast to the interface type 'Inventor.GeometryIntent'. This operation failed because a call to the QueryInterface method for the COM model component to retrieve an interface with IID identifier '{56B990B9-D25A-436F-A652-1D21EC739C57}' failed due to the following error: Such interface is not supported. (Exception from HRESULT: 0x80004002 (E_NOINTERFACE)).
PL:
Nie można rzutować obiektu modelu COM typu 'System.__ComObject' na typ interfejsu 'Inventor.GeometryIntent'. Ta operacja nie powiodła się, ponieważ wywołanie metody QueryInterface dla składnika modelu COM w celu uzyskania interfejsu o identyfikatorze IID '{56B990B9-D25A-436F-A652-1D21EC739C57}' nie powiodło się z powodu następującego błędu: Taki interfejs nie jest obsługiwany. (Wyjątek od HRESULT: 0x80004002 (E_NOINTERFACE)).

[bradeneuropeArthur]

I see your error is in the code?

[doma-zieman]

oDim2 = oGeneralDims.AddLinear(InsertPT, endPoint1 , endPoint2 , kHorizontalDimensionType)

oPt1 = oTG.CreatePoint2d(oView1.Left + (oView1.Width / 3), oView1.Top - oView1.Height - 1)

oView1 - is in place, it is on this sheet

X=20,4 Y=14,21

Dim endPoint2 As Point2d

X=10,4 Y=16,665

Dim endPoint1 As Point2d

X=30,4 Y=16,665

I do not know which ingredient cannot be dropped? Why can't it be dumped?

[duke]

When you say you want to dimension between two "planes", are you referring to work planes? Are these planes visible on your drawing? Drawing dimensions can only be placed between, or on, visible lines in the drawing. Work planes will very often cause errors because of how they are evaluated. Are there 2 faces that you can use instead? Faces are more reliable, and I can provide the code you would need to find named faces.

[doma-zieman]

No, they are called the faces of the element (appendix). They are visible.

[duke · Accepted solution]

Looking at your code, I believe your error may be that you didn't actually create a face proxy, you just referenced a face and attempted to apply the faceProxy type. Below is a code snippet that I use when I am automating dimensions. You see that I actually create and pass a face proxy.

Dim oComp as ComponentOccurrence
oComp = oModelDoc.ComponentDefinition.Occurrences(i)

'Locate the "FrontFace" face of the part
Dim FrontFace As Face = namedEntities.FindEntity("FrontFace")
	
'Create a geometry proxy to reference for the face
oComp.CreateGeometryProxy(FrontFace, oSketchProxy)

'Locate the associated curve in the drawing view
Dim oCurve As DrawingCurvesEnumerator = oBaseView.DrawingCurves(oSketchProxy)
	
Dim oIntent As GeometryIntent
oIntent = oSheet.CreateGeometryIntent(oCurve.Item(1))