Check for Disconnected Model in IDW

[MarkyTomm]

Hi All,

Quick question - is there a way to check for a disconnected model in an Inventor IDW

I want to scan through all sheets and if the model is disconnected (meaning that I have deleted it from the project) then delete that sheet.

Have my usual code snippet here - I may be using the wrong call by looking at the drawing view

Dim oDoc As DrawingDocument
Set oDoc = ThisApplication.ActiveDocument
Dim oView As DrawingView
On Error Resume Next
For Each oActiveSheet In oDoc.Sheets
oActiveSheet.Activate
Set oView = oDoc.ActiveSheet.DrawingViews(1)
*****Code here to check if the model is disconnected and delete the sheet if it is ********
Next

Any help, much appreciated

Regards

Mark

[JelteDeJong · Accepted solution]

You can try something like this:

Dim doc As DrawingDocument = ThisDoc.Document
Dim disconectedSheets As New List(Of Sheet)
For Each sheet As Sheet In doc.Sheets
    For Each view As DrawingView In sheet.DrawingViews
        If (view.ReferencedDocumentDescriptor.ReferencedDocument Is Nothing) Then
            disconectedSheets.Add(sheet)
        End If
    Next
Next

For Each sheet As Sheet In disconectedSheets
    sheet.Delete()
Next

[WCrihfield · Accepted solution]

Hi @MarkyTomm.  Looks like my response is a little slower, but it is in VBA, since your initial code seemed to be in VBA, and I don't use that much anymore.  You can give this version a try though, just in case it may work any better for you.  In this code I am checking if the 'reference is missing', instead of Is Nothing, because draft views may also not have a referenced document, and I did not know if you had any of those.

Sub DeleteSheetsWithMissingModelLinks()
	If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
		Call MsgBox("A Drawing document must be active for this code to work. Exiting.", vbCritical, "")
		Exit Sub
	End If
	Dim oDDoc As DrawingDocument
	Set oDDoc = ThisApplication.ActiveDocument
	Dim oSheets As Inventor.Sheets
	Set oSheets = oDDoc.Sheets
	Dim oSheet As Inventor.Sheet
	For Each oSheet In oSheets
		Dim oViews As DrawingViews
		Set oViews = oSheet.DrawingViews
		If oViews.Count = 0 Then Continue For
		Dim oView As DrawingView
		Set oView = oViews.Item(1)
		If oView.ReferencedDocumentDescriptor.ReferenceMissing Then
			oSheet.Delete
		End If
	Next
End Sub

[MarkyTomm]

Many tanks guys - going to go with the reference missing version coupled with the add sheet references to an array and delete at the end which I think will excute quickest. Will throw in an active sheet and user confirm dialogue just for checking. Will post the code here when finished. Have a good one!