Drawing properties to referenced models properties

[mikejones]

Hi all

I have a need to take a custom iproperty from a drawing; the drawing number in this case, and copy it to a custom iproperty called "Drawing" in all models  that are referenced in the drawing views. The views may contain an assembly drawing and a number of additional views of the component parts required for assembly. I'm not looking to go deeper than top level model in each of the views.  Any help appreciated.

Mike

[clutsa]

Give this iLogic a try

Dim app As Inventor.Application = ThisApplication
Dim doc As DrawingDocument = app.ActiveDocument
Dim docM As Document

For Each oView In doc.ActiveSheet.DrawingViews 'look at each view
	If oView.ParentView Is Nothing Then 'if it's a base view
		docM = oView.ReferencedFile.ReferencedDocument 'grab the base component
                'set the iProperty
		iProperties.Value(docM.DisplayName, "Custom", "Drawing") = iProperties.Value("Project", "Part Number")
	End If
Next

[mikejones]

Thanks for the reply but I'm getting an error message when I run it; see below

Error in rule: DrawingNumberToModel, in document: HGF1000 - 03-01-01 PHTM

Object reference not set to an instance of an object.

I know it's getting the model names ok because I put a message statement before the iProperties.Value statement so there must be something wrong with the line that is copying the iProperties over to the model.

Any ideas?

[clutsa · Accepted solution]

My guess is the display name has been overridden. Try this

Dim app As Inventor.Application = ThisApplication
Dim doc As DrawingDocument = app.ActiveDocument
Dim docM As Document

For Each oView In doc.ActiveSheet.DrawingViews 'look at each view
	If oView.ParentView Is Nothing Then 'if it's a base view
		docM = oView.ReferencedFile.ReferencedDocument 'grab the base component
                'set the iProperty
		docName = Right(docM.FullDocumentName, Len(docM.FullDocumentName) - InStrRev(docM.FullDocumentName,"\"))
		'MessageBox.Show(docName, "Title")

		iProperties.Value(docName, "Custom", "Drawing") = iProperties.Value("Project", "Part Number")
	End If
Next

[mikejones]

That is perfect, thanks Clutsa for your help. When I wrote some code myself I went along the same lines as the first lines you sent but without success, this new one works perfectly. I'm still not sure why the original code didn't work though

Thanks again

Mike

[clutsa]

Someone changed the display name of model... if it doesn't look like someone changed the display name they may have changed it buy typing the part number in as the display name. Slow click to edit the name, delete the entire name, then press enter and the default name will come back.