I’ve written some iLogic code to control the “View Style” and “View Representation” of drawing views. The code gathers all of the views in the drawing and presents them in a list to the user. It then presents a pre-defined set of “View Styles”, once it has done this, it then gathers all of the “View Representations” from the assembly model and presents these to the user.

The Animated GIF below shows the code in action (clicking on the GIF will open a higher resolution version in a new tab)

The user is able to select a drawing view, and then a “View Style” and “View Representation” to apply to the view. I’ve written some error handling into the code, to exit and make no changes if an initial view is not selected, and I have set defaults for instances where the user selects a view, but does not specify a “View Style” or “View Representation” The Animated GIF below shows the error handling / Default selections

The iLogic code is designed to work in drawings of Assembly models. If you run it in a Drawing of a part file the code will only give you the option to change the View Style.

Below is the iLogic Code, I have tried to comment it, so hopefully it will make sense to you. Special Thanks to Curtis Waguespack for some of the code he posted on a forum (credited in my code). Enjoy!

'iLogic code by @ClintBrown3D, originally posted at https://clintbrown.co.uk/control-drawing-view-reps-style-with-ilogic On Error GoTo ClintBrown3D '------------------------------------------VIEW SELECTION + SETUP ---------------------------------------- ' Iterate through drawing views & add to Array Dim oView As DrawingView = Nothing Dim oDrawingViews As DrawingViews = ThisApplication.ActiveDocument.Sheets.Item(1).DrawingViews Dim NewArrayList As New ArrayList For i = 1 To oDrawingViews.Count oView = oDrawingViews.Item(i) bView = oView.Name NewArrayList.Add(bView) Next ClintBrown3D = InputListBox("Choose a View", NewArrayList, d0, Title := "@ClintBrown3D", ListName := "Select a view to edit from the list below") If ClintBrown3D = "" Then : MessageBox.Show("No Selection made, Exiting", "@ClintBrown3D") : Return : End If 'Create Array & Input list box to choose view types Dim MyArrayList As New ArrayList MyArrayList.Add("Shaded") MyArrayList.Add("Hidden Line") MyArrayList.Add("Hidden Line Removed") MyArrayList.Add("Shaded Hidden Line") MyArrayList.Add("From Base Drawing View") ViewStyleType1 = InputListBox("Sets the View Style - Default is Hidden Line Removed. You are Editing: " & ClintBrown3D , MyArrayList, d0, Title := "@ClintBrown3D: " & ClintBrown3D, ListName := "Select a ''View Style'' from the list below") If ViewStyleType1 = "Shaded" Then : ViewStyleType = 32259 : End If If ViewStyleType1 = "Hidden Line" Then : ViewStyleType = 32257 : End If If ViewStyleType1 = "Hidden Line Removed" Then : ViewStyleType = 32258 : End If If ViewStyleType1 = "Shaded Hidden Line" Then : ViewStyleType = 32261 : End If If ViewStyleType1 = "From Base Drawing View" Then : ViewStyleType = 32260 : End If If ViewStyleType1 = "" Then : ViewStyleType = 32258 : MessageBox.Show("No selection made - ''View Style'' set to 'Hidden Line Removed'", "@ClintBrown3D") : End If '---------------------------------------------------------------- ---------------------------------------- '------------------------------------------VIEW REP CONTROLS + Curtis ------------------------------------ 'This section of Code adapted to work with drawings, based on code by Curtis Waguespack (original works in .iam files) ' on this forum >> https://forums.autodesk.com/t5/inventor-forum/ilogic-view-representations-toggling/td-p/6589121 Dim oAsmCompDef As AssemblyComponentDefinition oAsmCompDef = ThisDrawing.ModelDocument.ComponentDefinition Dim oViewReps As DesignViewRepresentations oViewReps = oAsmCompDef.RepresentationsManager.DesignViewRepresentations Dim oViewRep As DesignViewRepresentation Dim NameList As New ArrayList() For Each oViewRep In oViewReps NameList.Add(oViewRep.Name) Next '--------------------------------------------------------------------------------------------------------- NameList.Remove("Master") 'You can't select Master, so it is removed from the array If NameList.Count > 0 Then'This is to deal with drawings of parts ViewReptoActivate = InputListBox("Sets the View Rep - No selection sets view to ''Default'' View Rep. You are Editing: " & ClintBrown3D , NameList, d0, Title := "@ClintBrown3D: " & ClintBrown3D, ListName := "Select a View Rep from the list below") End If If NameList.Count = 0 Then : GoTo ApplyChanges : End If 'Give user feedback if nothing is selected (this is ignored in part files) If ViewReptoActivate = "" Then ViewReptoActivate = "Default" MessageBox.Show("No Selection made, view rep set to default", "@ClintBrown3D") End If '------------------------------------------APPLY CHANGES TO DRAWING--------------------------------------- ApplyChanges: ActiveSheet.View(ClintBrown3D).View.ViewStyle = ViewStyleType ActiveSheet.View(ClintBrown3D).View.SetDesignViewRepresentation(ViewReptoActivate, True) Return '--------------------------------------------------------------------------------------------------------- ClintBrown3D : Resume Next MessageBox.Show("OH SNAP! Something Has Gone Terribly WRONG :(", "@ClintBrown3D", MessageBoxButtons.OK, MessageBoxIcon.Asterisk, MessageBoxDefaultButton.Button1)

UPDATE 28 August 2019:

The Code above only works for the views on single sheets. Jerry Berns pointed out on Twitter that if you make a small tweak to the code, that you can use it on multi-sheet drawings.

Clint,

Thanks for sharing a very useful tool.👍 I changed the oDrawingViews line of code as follows: Dim oDrawingViews As DrawingViews = ThisApplication.ActiveDocument.ActiveSheet.DrawingViews This allows the active sheet views to be listed for a multi-sheet drawing. – Jerry — Jerry Berns (@JerryBerns) August 28, 2019

Clint,

Thanks for sharing a very useful tool.

I changed the oDrawingViews line of code as follows:

Dim oDrawingViews As DrawingViews = ThisApplication.ActiveDocument.ActiveSheet.DrawingViews

This allows the active sheet views to be listed for a multi-sheet drawing.

– Jerry