iLogic to Create Drawing with Flat Pattern View

[kara_johnsonLG2ZG]

Dim oCompDef As SheetMetalComponentDefinition
oCompDef = oDoc.ComponentDefinition
If oCompDef.HasFlatPattern = False Then
	MessageBox.Show("Please create flat pattern")
	Exit Sub
End If

Dim oDrawingDoc As DrawingDocument = ThisApplication.Documents.Add(DocumentTypeEnum.kDrawingDocumentObject,templateFile,True)

oDrawingDoc.Activate()
Dim oSheet As Sheet = oDrawingDoc.Sheets.Item(1)

Dim oView1, oView2, oView3 As DrawingView
Dim oTopRightPoint As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oSheet.Width * 2 / 3, oSheet.Height * 2 / 3)
Dim oLeftPoint As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oSheet.Width / 3, oSheet.Height / 2)

oView1 = oSheet.DrawingViews.AddBaseView(oDoc, oTopRightPoint, 1/8, ViewOrientationTypeEnum.kIsoTopRightViewOrientation, DrawingViewStyleEnum.kShadedDrawingViewStyle)
oView2 = oSheet.DrawingViews.AddBaseView(oDoc, oTopRightPoint, 1/8, ViewOrientationTypeEnum.kFlatBacksideViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle)
Dim oProjectedPoint As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oView2.Center.X, oView2.Center.Y -10)
oView3 = oSheet.DrawingViews.AddProjectedView(oView2, oProjectedPoint, DrawingViewStyleEnum.kFromBaseDrawingViewStyle)

I am creating an iLogic rule to automatically create drawings and place a couple of views. We are working with sheet metal and I would like to place a flat view. However, when I run my code, it says "the parameter is incorrect". I've narrowed this down to being the flat view orientation parameter (the red text). 

The ipt does have a flat pattern (and I also check if it has one in the code). If I try and edit the view that it does place (Iso Top Right), the flat pattern bubble is greyed out. But if I manually create a new base view, I can select flat pattern. 

Any ideas what I'm doing wrong?

[CGBenner]

@kara_johnsonLG2ZG 

Welcome to the Community!  I moved your post here because this is where all of the programmers hang out.  Good luck!

[patrick.schlambHPACQ · Accepted solution]

Dim oViewOptions As NameValueMap = ThisApplication.TransientObjects.CreateNameValueMap
oViewOptions.Add("SheetMetalFoldedModel", False)
oView2 = oSheet.DrawingViews.AddBaseView(oDoc, oTopRightPoint, 1/8, ViewOrientationTypeEnum.kBackViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle, AdditionalOptions := oViewOptions)
'oView2 = oSheet.DrawingViews.AddBaseView(oDoc, oTopRightPoint, 1/8, ViewOrientationTypeEnum.kFlatBacksideViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle)

 I have commented out your line and replaced it with a line I have used to successfully create flat pattern views in a drawing. I tried to match it to your existing code and variable, but may have missed something. Please let me know if this helps with your issue. 

[kara_johnsonLG2ZG]

Worked! Thank you so much for your help!