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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!
Solved! Go to Solution.
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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
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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
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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
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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
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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). ........
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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.
Or if this helped you, please, click (like)
Regards
Alan