Help about Deleting ONLY iLogic created dimensions from particular view or sheet

[sohaib.as01]

Hello Everyone, Greetings 🙂

I have created an iLogic code for my part which automatically created dimension when a rule is run for diemnsions creation using iLogic.

I have Inventor 2019 so I am using "Assign Name" functionality (similar to attribute manager add-in but much simpler) to create these dimensions.

Now each time the part is updated the dimension will be created between the two faces of the part, which is what I want.

Now I also want to delete the previously created iLogic dimensions because after each update o the part, previous dimension is staying their and new dimension is being added over it which obliviously i dont want.

I found this code in search of my answer but when I run this code, nothing happens whatsoever, not even an error is returned. So can someone please help me understand what is it I should do accomplish what I want?

Doc = ThisApplication.ActiveDocument
Dim Sheet As Inventor.Sheet
oSheet = Doc.ActiveSheet
'Iterate over all diemnsions
Dim oDim As GeneralDimension
For Each oDim In oSheet.DrawingDimensions
	If oDim.AttributeSets.NameIsUsed("iLogic_Created") = True Then
		oDim.Delete
	End If
	Next

Dim oDoc As Inventor.Document
oDoc = ThisApplication.ActiveDocument

Here is the code I am using to generate dimensions for the part, which is working as it should, in case someone needs it 🙂

Dim partDoc As PartDocument = ThisDoc.ModelDocument 'assinging variablr to active part documemnt
Dim namedEntities = iLogicVb.Automation.GetNamedEntities(partDoc) 'calling in all named faces in the active part doc
face0 = namedEntities.FindEntity("J_Face") 'assign named faces
face1 = namedEntities.FindEntity("J_end")

Dim oSheet = ThisApplication.ActiveDocument.ActiveSheet 'Assigning Variable to active sheet

Dim oView As DrawingView = ActiveSheet.View("VIEW1").View 'assign variable to active sheet

'Dim curve0 As DrawingCurvesEnumerator 'no idea why

curve0 = oView.DrawingCurves(face0) 'assign faces to variable as drawing curves
curve1 = oView.DrawingCurves(face1)

Dim finalCurve As DrawingCurve     'assigning a variable as drawing curve to store faces values
Dim finalCurve1 As DrawingCurve

'MessageBox.Show(curve1.Count.ToString)

finalCurve = curve0.Item(1)    'assigning curve faces values to variables
finalCurve1 = curve1.Item(1)

'MessageBox.Show(finalCurve1.ToString)

Dim oGeomIntent1 As GeometryIntent 'assigning a variable to geometry intent to use as annotations
Dim oGeomIntent2 As GeometryIntent

Dim oGeneralDims As GeneralDimensions = oSheet.DrawingDimensions.GeneralDimensions ' gaining acces to dimensioning in sheet

'oGeomIntent1 = oSheet.CreateGeometryIntent(finalCurve)
'oGeomIntent2 = oSheet.CreateGeometryIntent(finalCurve.EndPoint)
oGeomIntent1 = oSheet.CreateGeometryIntent(finalCurve) ' assigning drawing curve values to geometry variable 
oGeomIntent2 = oSheet.CreateGeometryIntent(finalCurve1)
Dim textPoint1 As Inventor.Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oView.Center.X - 6.5 , oView.Top)
'Dim textPoint2 As Inventor.Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oView.Center.X, oView.Top + .10)
oDim = oGeneralDims.AddLinear(textPoint1, oGeomIntent1, oGeomIntent2)
'oDim = oGeneralDims.AddLinear(textPoint2, oGeomIntent2)
'Dim linDim1 = genDims.AddLinear("Dimension 1", VIEW1.SheetPoint(0.5, -0.1),face1,Face2) Comapring code

[JhoelForshav · Accepted solution]

Hi @sohaib.as01 

In order to make the code to delete dimensions work, you'll need to add the attribute set "iLogic_Created" to the dimensions you create with your code. See code below, I just added the one line 🙂

Dim partDoc As PartDocument = ThisDoc.ModelDocument 'assinging variablr to active part documemnt
Dim namedEntities = iLogicVb.Automation.GetNamedEntities(partDoc) 'calling in all named faces in the active part doc
face0 = namedEntities.FindEntity("J_Face") 'assign named faces
face1 = namedEntities.FindEntity("J_end")

Dim oSheet = ThisApplication.ActiveDocument.ActiveSheet 'Assigning Variable to active sheet

Dim oView As DrawingView = ActiveSheet.View("VIEW1").View 'assign variable to active sheet

'Dim curve0 As DrawingCurvesEnumerator 'no idea why

curve0 = oView.DrawingCurves(face0) 'assign faces to variable as drawing curves
curve1 = oView.DrawingCurves(face1)

Dim finalCurve As DrawingCurve     'assigning a variable as drawing curve to store faces values
Dim finalCurve1 As DrawingCurve

'MessageBox.Show(curve1.Count.ToString)

finalCurve = curve0.Item(1)    'assigning curve faces values to variables
finalCurve1 = curve1.Item(1)

'MessageBox.Show(finalCurve1.ToString)

Dim oGeomIntent1 As GeometryIntent 'assigning a variable to geometry intent to use as annotations
Dim oGeomIntent2 As GeometryIntent

Dim oGeneralDims As GeneralDimensions = oSheet.DrawingDimensions.GeneralDimensions ' gaining acces to dimensioning in sheet

'oGeomIntent1 = oSheet.CreateGeometryIntent(finalCurve)
'oGeomIntent2 = oSheet.CreateGeometryIntent(finalCurve.EndPoint)
oGeomIntent1 = oSheet.CreateGeometryIntent(finalCurve) ' assigning drawing curve values to geometry variable 
oGeomIntent2 = oSheet.CreateGeometryIntent(finalCurve1)
Dim textPoint1 As Inventor.Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oView.Center.X - 6.5 , oView.Top)
'Dim textPoint2 As Inventor.Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oView.Center.X, oView.Top + .10)
oDim = oGeneralDims.AddLinear(textPoint1, oGeomIntent1, oGeomIntent2)

'Just add the attribute set to the dimension
oDim.AttributeSets.Add("iLogic_Created")
'oDim = oGeneralDims.AddLinear(textPoint2, oGeomIntent2)
'Dim linDim1 = genDims.AddLinear("Dimension 1", VIEW1.SheetPoint(0.5, -0.1),face1,Face2) Comapring code

If you run this rule and then run the rule to delete dimensions you posted It'll work 🙂

Doc = ThisApplication.ActiveDocument
Dim Sheet As Inventor.Sheet
oSheet = Doc.ActiveSheet
'Iterate over all diemnsions
Dim oDim As GeneralDimension
For Each oDim In oSheet.DrawingDimensions
	If oDim.AttributeSets.NameIsUsed("iLogic_Created") = True Then
		oDim.Delete
	End If
Next

[sohaib.as01]

Hey thank you so much @JhoelForshav your solution worked like a charm :)) I am a Mechanical Engineer, so not very good at programming, just remember stuff what i learned in University 😄

Can you also solve another final problem for me if you got time?

Now I want the same code to run for assembly, so I figured out this code from internet help and hit & trial. But its returning me an error "Object reference not set to an instance of an object".

I ran a Msg Box check to see which line is giving me this error; hence found out the line below

MessageBox.Show(check)

is giving me the error. So I suppose I am not calling the assembly part correctly? Also please note that I want a dimension between two same parts spaced apart , but for now I am just trying to get a dimension of just one face of the part to see if my code works correctly. Here is the code I am trying to run;

check = 2
Dim Doc As DrawingDocument
Doc = ThisDoc.Document 

Dim oAsmDoc As AssemblyDocument
Dim oCompDef As AssemblyComponentDefinition'assinging variable for component definations i assy

Dim FPColl As ObjectCollection
Dim OverallColl As ObjectCollection
Dim oText As Point2d
MessageBox.Show(check)
Dim S1 = oCompDef.Occurrences.ItemByName("J channel LED edge:1")
'Dim S2 = oCompDef.Occurrences.ItemByName("J Channel LED edge:2")

FPColl = ThisServer.TransientObjects.CreateObjectCollection
OverallColl = ThisServer.TransientObjects.CreateObjectCollection

Dim namedEntities = iLogicVb.Automation.GetNamedEntities(S1.Definition.Document)'calling in all named faces in the active part doc
'Dim namedEntities = iLogicVb.Automation.GetNamedEntities(S2.Definition.Document)

S1Face = namedEntities.FindEntity("J_Face") 'assign named faces
'face1 = namedEntities.FindEntity("J_end")

Dim oSheet = ThisApplication.ActiveDocument.ActiveSheet 'Assigning Variable to active sheet

Dim oView As DrawingView = ActiveSheet.View("FRONT").View 'assign variable to active sheet

Call S1.CreateGeometryProxy(S1Face, oSketchProxy)
Dim S1Curve = oView.DrawingCurves(oSketchProxy)

oIntent = oSheet.CreateGeometryIntent(S1Curve.Item(1))
Call OverallColl.Add(oIntent)

oText = ThisServer.TransientGeometry.CreatePoint2d(oView.Center.X - oView.Width / 2, oView.Center.Y - oView.Height / 2)

oText.Y = oText.Y - 1

Call oSheet.DrawingDimensions.GeneralDimensions.AddLinear(oText, OverallColl.Item(1)).CenterText

[JhoelForshav]

@sohaib.as01 

You're right that you never set a reference to the AssemblyDocument. The variables oAsmDoc and oCompDef are empty.

I think I understand from your code what you're trying to accomplish though so I wrote the code below for you with comments explaining all the operations. Hope it helps 🙂

'Get the drawing
Dim oDrawing As DrawingDocument = ThisDrawing.Document
'Get the active sheet
Dim oSheet As Sheet = oDrawing.ActiveSheet
'Get the view named "FRONT"
Dim oView As DrawingView
For Each drwView As DrawingView In oSheet.DrawingViews
	If drwView.Name = "FRONT"
		oView = drwView
		Exit For
	End If
Next
'Exit if view can't be found
If oView Is Nothing
	MsgBox("Couldn't find the drawing view named FRONT")
	Exit Sub
End If
'Get the assembly document from the view
Dim oAsm As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oCompDef As AssemblyComponentDefinition = oAsm.ComponentDefinition
Dim oOcc As ComponentOccurrence
'Get the occurrence named J channel LED edge:1
Try
oOcc = oCompDef.Occurrences.ItemByName("J channel LED edge:1")
Catch
'Exit if the occurrence can't be found
MsgBox("Couldn't find occurrence named J channel LED edge:1")
Exit Sub
End Try
'Get the named entities of J channel LED edge:1
Dim namedEntities = iLogicVb.Automation.GetNamedEntities(oOcc.Definition.Document)
Dim S1Face As Face
'Get the face named J_Face
Try
S1Face= namedEntities.FindEntity("J_Face")
Catch
'Exit if face cant be found
MsgBox("Couldn't find face named J_Face")
End Try
'Create a proxy object for the face
Dim S1FaceProx As FaceProxy
oOcc.CreateGeometryProxy(S1Face, S1FaceProx)
'Create geometry intent for the first drawingcurve segment of the curve representing the face.
Dim oIntent As GeometryIntent = oSheet.CreateGeometryIntent(oView.DrawingCurves(S1FaceProx)(1))
'Create a Point2d for the dimensions text position
Dim oText As Point2d = ThisApplication.TransientGeometry.CreatePoint2d _
(oView.Center.X - oView.Width / 2, oView.Center.Y - oView.Height / 2 - 1)
'Add the dimension
Dim oDim As LinearGeneralDimension = oSheet.DrawingDimensions.GeneralDimensions.AddLinear(oText, oIntent)
'Center the text
oDim.CenterText
'Add the attribute set to recognize that the dimension is placed by iLogic
oDim.AttributeSets.Add("iLogic_Created")

[sohaib.as01]

Thank you so very much @JhoelForshav your code worked perefectly well. I also expanded the code to take dismensions between two similar components with similar faces spaced apart and it also worked just fine. Many many thanks and appreciation that you took your precious time out to help me with my problem. 🙂

I am posting my code here in case someone else needs it for dimensioning.

Just one last question for you, I am wondering if the parts are in the sub-assembly of my main assy, then I suppose I am gonna have to call the sub-assy in the code, right? Any chance if you can tell me how to accomplish that? I have just one sub-assy in my main assy and the dimensions are gonna be between them actually, so the code only has to run a loop to find any sub assy it can and use its components to get faces.

'Get the drawing
Dim oDrawing As DrawingDocument = ThisDrawing.Document
'Get the active sheet
Dim oSheet As Sheet = oDrawing.ActiveSheet
'Get the view named "FRONT"
Dim oView As DrawingView
For Each drwView As DrawingView In oSheet.DrawingViews
	If drwView.Name = "FRONT"
		oView = drwView
		Exit For
	End If
Next
'Exit if view can't be found
If oView Is Nothing
	MsgBox("Couldn't find the drawing view named FRONT")
	Exit Sub
End If
'Get the assembly document from the view
Dim oAsm As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oCompDef As AssemblyComponentDefinition = oAsm.ComponentDefinition
Dim oOcc1 As ComponentOccurrence
Dim oOcc2 As ComponentOccurrence
'Get the occurrence named J channel LED edge:1
Try
oOcc1 = oCompDef.Occurrences.ItemByName("J channel LED edge:1")
oOcc2 = oCompDef.Occurrences.ItemByName("J channel LED edge:2")
Catch
'Exit if the occurrence can't be found
MsgBox("Couldn't find occurrence named J channel LED edge:1")
Exit Sub
End Try
'Get the named entities of J channel LED edge:1
Dim namedEntities1 = iLogicVb.Automation.GetNamedEntities(oOcc1.Definition.Document)
Dim namedEntities2 = iLogicVb.Automation.GetNamedEntities(oOcc2.Definition.Document)
Dim S1Face As Face
Dim S2Face As Face
'Get the face named J_Face
Try
S1Face = namedEntities1.FindEntity("J_Face")
S2Face = NamedEntities2.FindEntity("J_Face")
Catch
'Exit if face cant be found
MsgBox("Couldn't find face named J_Face")
End Try
'Create a proxy object for the face
Dim S1FaceProx As FaceProxy
Dim S2FaceProx As FaceProxy
oOcc1.CreateGeometryProxy(S1Face, S1FaceProx)
oOcc2.CreateGeometryProxy(S1Face, S2FaceProx)
'Create geometry intent for the first drawingcurve segment of the curve representing the face.
Dim oIntent1 As GeometryIntent = oSheet.CreateGeometryIntent(oView.DrawingCurves(S1FaceProx)(1))
Dim oIntent2 As GeometryIntent = oSheet.CreateGeometryIntent(oView.DrawingCurves(S2FaceProx)(1))
'Create a Point2d for the dimensions text position
Dim oText As Point2d = ThisApplication.TransientGeometry.CreatePoint2d _
(oView.Center.X - oView.Width / 2, oView.Center.Y - oView.Height / 2 - 1)
'Add the dimension
Dim oDim As LinearGeneralDimension = oSheet.DrawingDimensions.GeneralDimensions.AddLinear(oText, oIntent1, oIntent2)
'Center the text
oDim.CenterText
'Add the attribute set to recognize that the dimension is placed by iLogic
oDim.AttributeSets.Add("iLogic_Created")

[JhoelForshav]

Hi @sohaib.as01 

Just replace "SubAssemblyName" with the name of your subassembly and it should work 🙂

'Get the drawing
Dim oDrawing As DrawingDocument = ThisDrawing.Document
'Get the active sheet
Dim oSheet As Sheet = oDrawing.ActiveSheet
'Get the view named "FRONT"
Dim oView As DrawingView
For Each drwView As DrawingView In oSheet.DrawingViews
	If drwView.Name = "FRONT"
		oView = drwView
		Exit For
	End If
Next
'Exit if view can't be found
If oView Is Nothing
	MsgBox("Couldn't find the drawing view named FRONT")
	Exit Sub
End If
'Get the assembly document from the view
Dim oAsm As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oCompDef As AssemblyComponentDefinition = oAsm.ComponentDefinition
Dim oOcc1 As ComponentOccurrence
Dim oOcc2 As ComponentOccurrence
'Get the occurrence named J channel LED edge:1
Try
	'REPLACE "SubAssemblyName" with the name of your subassembly
	For Each oOcc As ComponentOccurrence In oCompDef.Occurrences.ItemByName("SubAssemblyName").SubOccurrences
		If oOcc.Name = "J channel LED edge:1" Then oOcc1 = oOcc
		If oOcc.Name = "J channel LED edge:2" Then oOcc2 = oOcc
	Next
	If oOcc1 Is Nothing Or oOcc2 Is Nothing
		MsgBox("Couldn't find the occurrences")
		Exit Sub
	End If
Catch
'Exit if the occurrence can't be found
MsgBox("Couldn't find SubAssembly")
Exit Sub
End Try
'Get the named entities of J channel LED edge:1
Dim namedEntities1 = iLogicVb.Automation.GetNamedEntities(oOcc1.Definition.Document)
Dim namedEntities2 = iLogicVb.Automation.GetNamedEntities(oOcc2.Definition.Document)
Dim S1Face As Face
Dim S2Face As Face
'Get the face named J_Face
Try
S1Face = namedEntities1.FindEntity("J_Face")
S2Face = namedEntities2.FindEntity("J_Face")
Catch
'Exit if face cant be found
MsgBox("Couldn't find face named J_Face")
End Try
'Create a proxy object for the face
Dim S1FaceProx As FaceProxy
Dim S2FaceProx As FaceProxy
oOcc1.CreateGeometryProxy(S1Face, S1FaceProx)
oOcc2.CreateGeometryProxy(S1Face, S2FaceProx)
'Create geometry intent for the first drawingcurve segment of the curve representing the face.
Dim oIntent1 As GeometryIntent = oSheet.CreateGeometryIntent(oView.DrawingCurves(S1FaceProx)(1))
Dim oIntent2 As GeometryIntent = oSheet.CreateGeometryIntent(oView.DrawingCurves(S2FaceProx)(1))
'Create a Point2d for the dimensions text position
Dim oText As Point2d = ThisApplication.TransientGeometry.CreatePoint2d _
(oView.Center.X - oView.Width / 2, oView.Center.Y - oView.Height / 2 - 1)
'Add the dimension
Dim oDim As LinearGeneralDimension = oSheet.DrawingDimensions.GeneralDimensions.AddLinear(oText, oIntent1, oIntent2)
'Center the text
oDim.CenterText
'Add the attribute set to recognize that the dimension is placed by iLogic
oDim.AttributeSets.Add("iLogic_Created")

[sohaib.as01]

okay @JhoelForshav got it, really appreciate you taking time out and helping me out. Cant thank you enough.

I was just wondering in this whole code we are hard coding the name of the components into the code, which is just perfect for me, to get faces, but I was wondering is there a way if we can tell the program to get say, 2nd or 3rd component from the model tree to get named entities? In that way we can make this code almost generic for every assembly. Or any other method similar to that? that will be wonderful, right?