Create Contour Flange

[meck]

Hi all

I've been trying to create a contour flange from a profile I've created with code. The really sad part is I'm not sure if the profile is even valid.

oProfile = oSketch.Profiles.AddForSurface

Is AddForSurface the proper profile to use when creating a contour flange?

I'm not even sure how to get from the profile to the feature to create the contour flange.

Any help would be greatly appreciated!

[meck]

Further explanation:

Using iLogic I create an open profile with code. It's the first sketch in the sheet metal part file. I wish to create a contour flange from that profile.

In the Inventor help, the examples of sheet metal flanges reference faces and edges. In my case I have neither the faces nor edges, unless it is considering the entities in the profile the edges. In a nut shell I cannot find any way to get from the sketch profile to the flange feature.

Here is all the code I have...

    Dim sheetMetalDoc As PartDocument
     sheetMetalDoc = ThisDoc.Document
 
    Dim smCompDef As SheetMetalComponentDefinition
    smCompDef = sheetMetalDoc.ComponentDefinition

    Dim profile As profile
    profile = oSketch.Profiles.AddForSolid

I hope this helps clarify my problem.

[Vladimir.Ananyev · Accepted solution]

Could you please try the following VBA code sample:

Sub Test()
    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument
    
    Dim oDef As SheetMetalComponentDefinition
    Set oDef = oDoc.ComponentDefinition
    
    Dim oSketch As PlanarSketch
    Set oSketch = oDef.Sketches.Item(1)
    
    ' Create a path.
    Dim oPath As Path
    Set oPath = oDef.Features.CreatePath(oSketch.SketchLines.Item(1))
    
    Dim oContourFlangeFeatures As ContourFlangeFeatures
    Set oContourFlangeFeatures = oDef.Features.ContourFlangeFeatures

    ' Create the flange definition.
    Dim cfDef As ContourFlangeDefinition
    Set cfDef = oContourFlangeFeatures.CreateContourFlangeDefinition(oPath)
    'set the distance extent
    Call cfDef.SetDistanceExtent(5, PartFeatureExtentDirectionEnum.kSymmetricExtentDirection)
    
    Dim oCF As ContourFlangeFeature
    Set oCF = oContourFlangeFeatures.Add(cfDef)

End Sub

Hope this helps.

[meck]

Thanks Vladimir it worked great!