[iLogic] Acessing Model Component Definition From Drawing

[JoãoASilva]

Hello All!

I'm trying to acess the Sheet Metal Component Definition of the model displayed on a drawing, but every way I try returns an error.

What I need:

I need a rule to check if the sheetmetal has any type of bends.

If it has, then → iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"

If it doesn't → iProperties.Value("Summary", "Comments") = "Laser Cut"

What I have:

I have a rule inside a sheetmetal template that runs with a "before saving" trigger.

Dim smDef As SheetMetalComponentDefinition = ThisDoc.Document.ComponentDefinition
Dim pf As PartFeature

'set our custom properties to "Laser Cut" to start with..
iProperties.Value("Summary", "Comments") = "Laser Cut"

'loop through each part feature
For Each pf In smDef.Features
	If pf.Suppressed = False Then

		If TypeOf pf Is FlangeFeature Then
		iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"
		End If
		
		If TypeOf pf Is ContourFlangeFeature Then
		iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"
		End If
		
		If TypeOf pf Is HemFeature Then
		iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"
		End If
		
		If TypeOf pf Is FoldFeature Then
		iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"
		End If

	End If
Next

What I want:

I want to check for bends on older sheetmetal parts were this rule wasn't yet implemented.

For this, I was considering acessing the part features thru the drawing.

All my drawings have multisheets.

Also, a few colleagues create sheetmetal parts by converting normal parts (I know this causes the SubType to be different from an originally created sheetmetal); sometimes they don't even convert, so they stay as "part".

For this reason, I want to filter when the rule runs using our coding scheme, wich I know how to do.

What I know:

I know how to go thru each and every sheet and fire rules based on the "in view model" subtype or part number.

My current code:

'['get full name of the model in the first view
Dim aDoc As DrawingDocument 
aDoc = ThisApplication.ActiveDocument

Dim aSheet As Sheet
Dim aViews As DrawingViews
Dim aView As DrawingView

aSheet = ActiveSheet.Sheet

aViews = aSheet.DrawingViews

If aViews.Count > 0 Then
	aView = aViews.Item(1)
	aModelFullName = aView.ReferencedDocumentDescriptor.ReferencedDocument.DisplayName
End If']
	
'['Part variables
Dim oPart As PartDocument
Dim oPartPath As String
Dim FulloPartName As String
	
' Set a reference to the target part
FulloPartName = ThisDoc.Path
FulloPartName = FulloPartName & "\" & aModelFullName
oPart = ThisApplication.Documents.ItemByName(FulloPartName)
']
	
ThisApplication.Documents.Open(FulloPartName)
	
'['Check Bend
Dim smDef As SheetMetalComponentDefinition = ThisDoc.Document.ComponentDefinition
Dim pf As PartFeature

'set our custom properties to "Laser Cut" to start with..
iProperties.Value("Summary", "Comments") = "Laser Cut"

'loop through each part feature
For Each pf In smDef.Features
	If pf.Suppressed = False Then
		
		If TypeOf pf Is FlangeFeature Then
		iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"
		End If
		
		If TypeOf pf Is ContourFlangeFeature Then
		iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"
		End If
		
		If TypeOf pf Is HemFeature Then
		iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"
		End If
		
		If TypeOf pf Is FoldFeature Then
		iProperties.Value("Summary", "Comments") = "Laser Cut + Bending"
		End If
		
	End If
Next']
	
oPart.Close

 The problem occurs on the " '['Check Bend " part.

What I have tried:

I replaced the "Check Bend" with a message box and everything else works.

I tried to run the "Check Bend" as an external rule, but to no avail.

Maybe I'm missing a simple detail or it just can't be done this way.

Any tips?

[J-Camper]

I think you need to change this line:

Dim smDef As SheetMetalComponentDefinition = ThisDoc.Document.ComponentDefinition

Because with the new rule "ThisDoc.Document" is a drawing document.  You should be accessing your "oPart" Object:

Dim smDef As SheetMetalComponentDefinition = oPart.ComponentDefinition

But you will probably want to verify the "oPart" from the view is a sheet metal part or the above line will fail.

[WCrihfield · Accepted solution]

Maybe try it this way:

Dim oDDoc As DrawingDocument = ThisDrawing.Document
Dim oPDoc As PartDocument
Dim oSMDef As SheetMetalComponentDefinition
Dim oSMFeats As SheetMetalFeatures
For Each oSheet As Inventor.Sheet In oDDoc.Sheets
	If oSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kPartDocumentObject Then
		oPDoc = oSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
		If oPDoc.PropertySets.Item("Design Tracking Properties").Item("Document SubType Name").Value = "Sheet Metal" Then
			oSMDef = oPDoc.ComponentDefinition
			oSMFeats = oSMDef.Features
			If oSMFeats.FlangeFeatures.Count > 0 Or _
				oSMFeats.ContourFlangeFeatures.Count > 0 Or _
				oSMFeats.HemFeatures.Count > 0 Or _
				oSMFeats.FoldFeatures.Count > 0 Then
				oPDoc.PropertySets.Item("Inventor Summary Information").Item("Comments").Value = "Laser Cut + Bending"
			End If
		Else 'it's a regular part (not sheet metal)
			oPDoc.PropertySets.Item("Inventor Summary Information").Item("Comments").Value = "Laser Cut"
		End If
	'Else ' the model in the drawing view is not a part document, so do nothing, then next.
	End If
Next

[JoãoASilva]

I tried that but didn't work as well.

But ty for your help!

[JoãoASilva]

I added a case to your working code and now it covers all my cases!

Before accepting as a solution, is there a simple way to make this code only applicable to one sheet?

That way I could just insert it in my fully functional "big macro", and run when the coding applies.

Ty!

[WCrihfield · Accepted solution]

OK. Try this then.

Dim oDDoc As DrawingDocument = ThisDrawing.Document
Dim oSheet As Inventor.Sheet = oDDoc.ActiveSheet
Dim oPDoc As PartDocument
Dim oSMDef As SheetMetalComponentDefinition
Dim oSMFeats As SheetMetalFeatures
If oSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kPartDocumentObject Then
	oPDoc = oSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
	If oPDoc.PropertySets.Item("Design Tracking Properties").Item("Document SubType Name").Value = "Sheet Metal" Then
		oSMDef = oPDoc.ComponentDefinition
		oSMFeats = oSMDef.Features
		If oSMFeats.FlangeFeatures.Count > 0 Or _
			oSMFeats.ContourFlangeFeatures.Count > 0 Or _
			oSMFeats.HemFeatures.Count > 0 Or _
			oSMFeats.FoldFeatures.Count > 0 Then
			oPDoc.PropertySets.Item("Inventor Summary Information").Item("Comments").Value = "Laser Cut + Bending"
		End If
	Else 'it's a regular part (not sheet metal)
		oPDoc.PropertySets.Item("Inventor Summary Information").Item("Comments").Value = "Laser Cut"
	End If
'Else ' the model in the drawing view is not a part document, so do nothing, then next.
End If

[JoãoASilva]

Your first answer was more than what I wanted, but was correct.

The second one is exactly what I needed.

Thank you!