iLogic drawing view controls in drawing files

[tonychristman4915]

Hello all,

I'm looking for how to use inventor iLogic to activate and deactivate the "Definition in Base View" option for drawing views. This is found by double clicking on a drawing view and selecting the "Display Options" tab.

I have a drawing file that uses an iLogic rule to activate and place section views but I want to give the option to our engineering staff to change the locations of the section views, then run a rule that hides all the arrows that clog up the Base view without having to click on every view manually.

The closest post I've found was this one: http://forums.autodesk.com/t5/inventor-general-discussion/ilogic-make-drawing-view-shaded/td-p/37586... that discussed how to use iLogic to change the view style, however I haven't discovered how to control the "Definiton in Base View" option yet.

Thanks!

[Curtis_Waguespack]

Hi tonychristman4915,

Here's a quick example based on the one at the link you provided.

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

Dim oDrawDoc As DrawingDocument
 oDrawDoc = ThisApplication.ActiveDocument

Dim oSheet As Sheet
oSheet = oDrawDoc.ActiveSheet

' select drawing views on active sheet
Dim oDrawView As DrawingView

For Each oDrawView In oSheet.DrawingViews	
	'adjust drawing view
	If oDrawView.ViewType = DrawingViewTypeEnum.kDetailDrawingViewType Then
		'toggle detail view fence visiblility
		If oDrawView.DisplayDefinitionInBase = False Then
		oDrawView.DisplayDefinitionInBase = True
		Else
		oDrawView.DisplayDefinitionInBase = False
		End If
	End If
Next

' **** DrawingViewTypeEnums ****
'	kAssociativeDraftDrawingViewType = 10506 
'	kAuxiliaryDrawingViewType = 10499 
'	kCustomDrawingViewType = 10498 
'	kDefaultDrawingViewType = 10497 
'	kDetailDrawingViewType = 10502  
'	kDraftDrawingViewType = 10505 
'	kOLEAttachmentDrawingViewType = 10500  
'	kOverlayDrawingViewType = 10507 
'	kProjectedDrawingViewType = 10504 
'	kSectionDrawingViewType = 10503 
'	kStandardDrawingViewType = 10501 

[Curtis_Waguespack · Accepted solution]

Here's another example that turns off sections arrows/lines for sections views:

Dim oDrawDoc As DrawingDocument
 oDrawDoc = ThisApplication.ActiveDocument

Dim oSheet As Sheet
oSheet = oDrawDoc.ActiveSheet

' select drawing views on active sheet
Dim oDrawView As DrawingView

For Each oDrawView In oSheet.DrawingViews	
	'look for section views
	If oDrawView.ViewType = DrawingViewTypeEnum.kSectionDrawingViewType Then
		'turn off section view annotations
		oDrawView.DisplayDefinitionInBase = False
	End If
Next

[tonychristman4915]

This worked perfectly and was exactly what I was looking for. Thanks!

[LSKELLY]

Hi Curtis

I have been looking for a way to change the Model State of a DrawingView object. I can't find any settings in the object browser. Any chance I am missing it under an obscure name?

I half expect it to look something like: 

Dim oDrawView As DrawingView
oDrawView.ModelState = "Machining" 

Lance Skelly

[LSKELLY]

Don't worry I found it. The following snippet illustrates how to change the Model State of a weldment view.

'Create View
oBaseView = oSheet.DrawingViews.AddBaseView(oPartDoc, oPoint1, ViewScale, ViewOrientationTypeEnum.kIsoTopRightViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle)
                
'View Settings
oBaseView.DisplayForeshortenedTangentEdges = True
If oPartDoc.DocumentSubType.DocumentSubTypeID = "{28EC8354-9024-440F-A8A2-0E0E55D635B0}" 'If Weldment
    oBaseView.SetWeldmentState(WeldmentStateEnum.kMachiningWeldmentState)
End If

[dbushDQ3RE]

HI Guts,

Making the view is one thing, put how do I access the (Welds Model State) and the (Welds components) in that view to Make Dimensions on named Faces using ILogic. I can make Dimensions for the (Assembly Model State) and its Components). ........

[A.Acheson]

Hi @dbushDQ3RE 

I would suggest to make a new post as this original post is solved and relates to a very generic question "iLogic drawing view controls in drawing files"

Your question relates to multiple questions each likely deserving its own post due to there complications.