Change Design View in IDW

[Anonymous]

Hi,

Change Design View in IDW.

Followupfrom a thread from Years ago..

Lookin got get designViewrep name in Drawing FIle.

Sub DesignViewRep()

    Dim oDoc As DrawingDocument
    Set oDoc = ThisApplication.ActiveDocument
    
    Dim oDrawingView As DrawingView
    Set oDrawingView = ThisApplication.CommandManager.Pick(kDrawingViewFilter, "Select a drawing view")
    
    MsgBox oDrawingView.ActiveDesignViewRepresentation

End Sub

Above macro from Daniel is not working.. please fing avi file attached.

hope we will get some soloution for a simple and small issue.

[Anonymous]

What Inventor version are you using? I tested the code with Inventor 2013. See below for a section from the programming help. I looks like it's in the API since Inventor 11.

What is the problem with the code? do you get a runtime error or just an empty msgbox?

DrawingView.ActiveDesignViewRepresentation Property

Parent Object: DrawingView

Description

Property that returns the name of the active Design View Representation for a drawing view of an assembly. This property returns a null string for drawing views of parts & presentations and in the case where the model (assembly) is unresolved.

Syntax

DrawingView.ActiveDesignViewRepresentation() As String

Version

Introduced in Inventor version 11

[Anonymous]

Hii..

It is just retuning an empty MsgBox. If you have any File Transfer (large file) I can send you debug video.

Just an Empty Msgbox. Nothing else.No errors.

[Anonymous]

Are you selecting an assembly view?

This line in the help will explain the empty message box: "This property returns a null string for drawing views of parts & presentations and in the case where the model (assembly) is unresolved."

[Anonymous]

That is a clean and simple Assembly, And I am selecting the viewas well.

Is that working with oyu?? Iam Using INV 2013.

[Anonymous]

Hmm last week it worked, but I now seem to get the same behavior you mention. Just an empty msgbox.

I will try to find out what the problem is.

Daniël

[Anonymous]

Ok, here's what I've found out.

When I place a view with a design view other than Master selected, the code works. If I select another design view other than master, the code also works. But if I select the master design view, the ActiveDesignViewRepresentation property returns an emptry string. Even more strange, when I now select another design view (which previously worked), the string is still empty!

Could you please check if you can reproduce this?

[Anonymous]

ActiveDesignViewRepresentation  property works if and only Associative box is checked (marked) when placing the view on the drawing sheet.

But I am looking to get the name of the view even if assocative is not selected.

Even if there is a custom view (or Default View), without associative checked, msgbox result a null value.

May be somebody should fix or clarify.

[xiaodong_liang]

Hi,

this is a known issue which has been logged: ActiveDesignViewRepresentation  should return the corresponding view name no matter the view associative or not.

[Crstiano]

Hi Xiaodong,

I have similar problem... my ActiveDesignViewRepresentation always returns = ""

Exist a correct way for control and change the DesignViewRepresentation of the SubAssembly in the Assembly?

I try in IV2014, if I use:

Call oOcc.SetDesignViewRepresentation ("OffZones")

 The software crash !!!!

If I use:

Dim oRepMan As RepresentationsManager
Set oRepMan = oOcc.Definition.RepresentationsManager
Dim oDVR As DesignViewRepresentation
Set oDVR = oRepMan.DesignViewRepresentations.Item("OffZones")
Call oDVR.Activate

 Don't show effects....

And another set: How define IsAssociativeToDesignViewRepresentation in this change ??

Thanks in advance