iLogic error with folding sheet metal

[SharkDesign]

I am using the following code to automatically create a flat pattern when I save a sheet metal document.

Dim oDoc As PartDocument
oDoc = ThisApplication.ActiveDocument
Dim State As SheetMetalComponentDefinition
State=oDoc.ComponentDefinition
If State.HasFlatPattern = False Then
State.Unfold 
End If

The problem comes when I insert this part into an assembly. When the sheet metal part has been edited and I save the assembly I get the following error:

Error in rule: unfold, in document: Part19.ipt

Unable to cast COM object of type 'Inventor._DocumentClass' to interface type 'Inventor.PartDocument'. This operation failed because the QueryInterface call on the COM component for the interface with IID '{29F0D463-C114-11D2-B77F-0060B0F159EF}' failed due to the following error: No such interface supported (Exception from HRESULT: 0x80004002 (E_NOINTERFACE)).

More Info tab:

System.InvalidCastException: Unable to cast COM object of type 'Inventor._DocumentClass' to interface type 'Inventor.PartDocument'. This operation failed because the QueryInterface call on the COM component for the interface with IID '{29F0D463-C114-11D2-B77F-0060B0F159EF}' failed due to the following error: No such interface supported (Exception from HRESULT: 0x80004002 (E_NOINTERFACE)).

at LmiRuleScript.Main()

at Autodesk.iLogic.Exec.AppDomExec.ExecRuleInAssembly(Assembly assem)

at iLogic.RuleEvalContainer.ExecRuleEval(String execRule)

Any ideas?

[Curtis_Waguespack]

Hi jameswillo,

Give this a try.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

'Loop through any and all referenced documents
For Each oDoc In ThisApplication.ActiveDocument.AllReferencedDocuments	
	'look at only sheet metal parts
	If oDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
	
		Dim State As SheetMetalComponentDefinition
		State = oDoc.ComponentDefinition
		
		If State.HasFlatPattern = False Then
			'create flat pattern
			State.Unfold 
			
			'flip back to folded model	
			State.FlatPattern.ExitEdit	
			
			'close the file
			oDoc.Close(True) 'True skips the save 
			
		End If
	End If
Next

'update assembly
InventorVb.DocumentUpdate()

[SharkDesign]

I'm assuming you put this code in the assembly rather than the part?

Am I right in thinking that if my assembly is very large this will massively increase my save time if it's going through every sheet metal part?

[adam.nagy]

Hi,

If the rule is triggered when the assembly is active then this is the part that will fail causing error "Unable to cast COM object of type 'Inventor._DocumentClass' to interface type 'Inventor.PartDocument'" because it's an assembly document:

oDoc = ThisApplication.ActiveDocument

Instead, you should work with the document that the rule resides in:

oDoc = ThisDoc.Document

Cheers, 

[SharkDesign]

Ahhhh, that makes sense. Thanks, I'll try that.