Autodesk Inventor Customization

[#1]

HI

I am after help on some ilogic code ,I have had some code done to isolate selected parts in a assembly file that has a specific custom property filled in i.e. : DESC2.It then creates view reps and locks down giving the rep name the same name as part.

What I am after if any one can help is some code that will place these isolated view reps as views on my dwg that the assembly resides in.With the functionality of picking face to show plan view of parts.

Any thoughts would be appreciated.

Dave

[#2]

Hi,

If I understand correctly, you want to place the drawing views from one assembly in specific view reps (or even specific LOD etc) like UI does (see attachment). If yes, you could use Advanced API of ilogic to access Inventor API. DrawingViews.AddBaseView allows you to specify additional or advanced options:

Name	Value Type	Valid Document Type
WeldmentFeatureGroup	WeldmentFeatureGroupEnum	Weldment
SheetMetalFoldedModel	Boolean	Sheet Metal
DesignViewRepresentation	String	Part, Assembly
DesignViewAssociative	Boolean	Part, Assembly
PositionalRepresentation	String	Assembly
MemberName	String	Part, Assembly
PresentationView	String	Presentation
PresentationViewAssociative	Boolean	Presentation

Following is a demo code I converted from the sample in the help reference of Inventor API:

' Set a reference to the drawing document. 
' This assumes a drawing document is active. 
Dim oDrawDoc As DrawingDocument 
oDrawDoc = ThisApplication.ActiveDocument 

'Set a reference to the active sheet. 
Dim oSheet As Sheet 
oSheet = oDrawDoc.ActiveSheet 

' Create a new NameValueMap object 
Dim oBaseViewOptions As NameValueMap 
oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap 

' Set the representations to use when creating the base view. 
'Call oBaseViewOptions.Add("PositionalRepresentation", "MyPositionalRep") 
Call oBaseViewOptions.Add("DesignViewRepresentation", "Default") 
'Call oBaseViewOptions.Add("DesignViewAssociative", True) 

' Open the model document (corresponding to the "MyLODRep" representation). 
Dim strFullDocumentName As String 
strFullDocumentName = ThisApplication.FileManager.GetFullDocumentName("c:\temp\reps.iam", "Master") 

Dim oModel As Document 
oModel = ThisApplication.Documents.Open(strFullDocumentName, False) 


' Create the placement point object. 
Dim oPoint As Point2d 
oPoint = ThisApplication.TransientGeometry.CreatePoint2d(25, 25) 

' Create a base view. 
Dim oBaseView As DrawingView 
 oBaseView = oSheet.DrawingViews.AddBaseView(oModel, oPoint, 2, _ 
kIsoTopLeftViewOrientation, kHiddenLineRemovedDrawingViewStyle, _ 
, , oBaseViewOptions)