Inventor drawing: Access view tree to toggle hidden lines for certain parts

[Mario.van.der.raaf]

I am trying to set hidden lines for the following component in my view: VIEW1, 000076253.iam, N1 + N3, 000078783:1.

So far i have had no succes in selecting anything with iLogic past the view.

I want to show hidden lines for 000078783:1 automatically.

The reason why i need to do this is so that the component shows up on the drawing view. My model is parametric so for some configurations 000078783 is not visible, if it becomes visible in a later configuration hidden lines are off again. So i need a way to toggle them if needed.

I found a way to target the modeldocument behind a view, but i am not certain how to proceed:

Dim oSheet As Sheet = ThisDoc.Document.ActiveSheet
Dim oView As DrawingView = oSheet.DrawingViews.Item(1) ' Specify the view name
Dim modelDocument As Document = oView.ModelDocument

Any help or links to the documentation would be greatly appreciated!

[WCrihfield]

Hi @Mario.van.der.raaf.  What you are wanting to do is a somewhat complicated, and highly custom task to automate.  One of the main tools for accomplishing what you want to do is the DrawingView.DrawingCurves property, which acts a bit like a Function.  You can supply a model object as input, and it will return the geometry objects currently visible within that view for that object (if any).  But before you can effectively use it, you will first need to get a reference to the model geometry needed as the input.  Once you have a reference to the model document object that is referenced within the DrawingView, you can then proceed to dig down within its ComponentDefinition.Occurrences collection, to access the specific ComponentOccurrence (or ComponentOccurrenceProxy) object, and set that as the value of that type of a ComponentOccurrence type variable.  Once you have that, you can use it in that DrawingCurves property to get the DrawingCurvesEnumerator collection representing the DrawingCurves within that view which represent that component.  Then you can loop through those DrawingCurve objects, and may also need to loop through the DrawingCurveSegment objects within each DrawingCurve object to change them.  You can either change them individually, which often takes longer to process, and is more difficult to change again later if needed.  Or you can collect each of them into an ObjectCollection, then use the Sheet.ChangeLayer method to change them all to a specific layer at once, which is set-up the way you want it.

By the way, the standard API way to access the model document being referenced by a DrawingView is like this:

Dim oViewDoc As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument

[Curtis_Waguespack · Accepted solution]

Hi @Mario.van.der.raaf 

If you're trying to set this check box, then this example might work.

Sub Main
	aVName = "VIEW1"
	sCompName = "000078783:1"

	Dim oDrawingDoc As DrawingDocument
	oDrawingDoc = ThisApplication.ActiveDocument

	Dim oSheet As Sheet = oDrawingDoc.ActiveSheet

	For Each oView In oSheet.DrawingViews
		If oView.Name = aVName Then

			'Get the browser node definition of the drawing view
			Dim oNativeBrowserNodeDef As NativeBrowserNodeDefinition
			oNativeBrowserNodeDef = oDrawingDoc.BrowserPanes.GetNativeBrowserNodeDefinition(oView)

			'Get the top browser node
			Dim oTopBrowserNode As BrowserNode
			oTopBrowserNode = ThisApplication.ActiveDocument.BrowserPanes.ActivePane.TopNode

			' Get the browser node of the view 
			Dim oNode As BrowserNode
			oNode = oTopBrowserNode.AllReferencedNodes(oNativeBrowserNodeDef).Item(1)

			Call recurseNodes(oNode, sCompName)
			Exit Sub
		End If
	Next oView

End Sub


Sub recurseNodes(node As BrowserNode, sName As String)

	'See if the node label is the name of the component
	If node.BrowserNodeDefinition.Label = sName Then
		'Expand the node 
		Try : node.Expanded = True: Catch : End Try

		'Select the node 
		node.DoSelect()

		CmdMan = ThisApplication.CommandManager
		CmdMan.ControlDefinitions.Item("DrawingBodyHiddenLinesCtxCmd").Execute

		NodeFound = True
	End If

	If NodeFound = True Then Exit Sub

	Dim bn As BrowserNode
	For Each bn In node.BrowserNodes
		If NodeFound = False Then
			Try
				If Not TypeName(bn.NativeObject) = "DrawingView" Then
					Call recurseNodes(bn, sName)
				End If
			Catch
				Exit Sub
			End Try
		End If
	Next
End Sub

 I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Mario.van.der.raaf]

Thanks for all the replies, what I did in the end is create a new part which changes dimensions using iLogic to suite my entire model range. This way I could leave the part active and prevent it from resetting the hidden lines feature. This proved easier and solved another issue my previous approach had, which was that the part i wanted to show had a lot of internal feature which would make the drawing messy.