Inventor Customization

Valued Contributor
Posts: 70
Registered: ‎03-26-2008
Message 1 of 4 (510 Views)

Ilogic View Reps on dwg

510 Views, 3 Replies
12-19-2012 10:37 PM



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.






ADN Support Specialist
Posts: 1,272
Registered: ‎06-12-2011
Message 2 of 4 (459 Views)

Re: Ilogic View Reps on dwg

01-14-2013 08:25 PM in reply to: dclunie



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:


Value Type 
Valid Document Type 
Sheet Metal 
Part, Assembly 
Part, Assembly 
Part, Assembly 


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) 


Xiaodong Liang
Developer Technical Services
Autodesk Developer Network

Distinguished Contributor
Posts: 178
Registered: ‎04-30-2012
Message 3 of 4 (259 Views)

Re: Ilogic View Reps on dwg

09-18-2013 03:25 AM in reply to: dclunie

Anybody know to take the designviewreprentation, to see if is a front, side, top view in a drawing?

same to that

CurrentOrientation = activesheet.View("View1").DesignViewRepresentation


Thnaks for your help!

Distinguished Contributor
Posts: 178
Registered: ‎04-30-2012
Message 4 of 4 (195 Views)

Re: Ilogic View Reps on dwg

10-25-2013 05:44 AM in reply to: sergelachance

Ok i have now :smileyhappy:


Dim odoc As DrawingDocument
odoc = ThisApplication.ActiveDocument
Dim tmpView As DrawingView

'Which text for which orientation
Select Case tmpView.Camera.ViewOrientationType
Case ViewOrientationTypeEnum.kBackViewOrientation
iProperties.Value("Custom", "TEST") = "Back View"
Case ViewOrientationTypeEnum.kBottomViewOrientation
iProperties.Value("Custom", "TEST")= "Bottom View"
Case ViewOrientationTypeEnum.kFrontViewOrientation
iProperties.Value("Custom", "TEST") = "Front View"
Case ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation
iProperties.Value("Custom", "TEST") = "Iso - Bottom Left View"
Case ViewOrientationTypeEnum.kIsoBottomRightViewOrientation
iProperties.Value("Custom", "TEST")= "Iso - Bottom Right View"
Case ViewOrientationTypeEnum.kIsoTopLeftViewOrientation
iProperties.Value("Custom", "TEST") = "Iso - Top Left View"
Case ViewOrientationTypeEnum.kIsoTopRightViewOrientation
iProperties.Value("Custom", "TEST")= "Iso - Top Right View"
Case ViewOrientationTypeEnum.kLeftViewOrientation
iProperties.Value("Custom", "TEST") = "Left View"
Case ViewOrientationTypeEnum.kRightViewOrientation
iProperties.Value("Custom", "TEST")= "Right View"
Case ViewOrientationTypeEnum.kTopViewOrientation
iProperties.Value("Custom", "TEST") = "Top View"
Case Else
iProperties.Value("Custom", "TEST") = ""
End Select

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