[Bug?] ClientFeature error when its definition includes a CombineFeature

[nnikbin]

It seems that when a ClientFeatureDefinition includes a CombineFeature, ClientFeature.Add method produces an error. And it seems that there is a history related to this issue (Link).

For example, the following code works fine, but if we comment out line 53 and uncomment line 56, it produces an error (see the image)

Public Sub TestClientFeature()

    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.Documents.Add(kPartDocumentObject, _
                ThisApplication.FileManager.GetTemplateFile(kPartDocumentObject))

    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oPartDoc.ComponentDefinition

    Dim oSketch As PlanarSketch
    Set oSketch = oCompDef.Sketches.Add(oCompDef.WorkPlanes.Item(3))

    Dim oTransGeom As TransientGeometry
    Set oTransGeom = ThisApplication.TransientGeometry

    Dim oCircle As SketchCircle
    Set oCircle = oSketch.SketchCircles.AddByCenterRadius(oTransGeom.CreatePoint2d(0, 0), 1)

    Dim oPaths As ObjectCollection
    Set oPaths = ThisApplication.TransientObjects.CreateObjectCollection
    oPaths.Add oCircle
    
    Dim oProfile As Profile
    Set oProfile = oSketch.Profiles.AddForSolid(False, oPaths)

    Dim oExtrudeDef As ExtrudeDefinition
    Set oExtrudeDef = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kNewBodyOperation)
    Call oExtrudeDef.SetDistanceExtent(1, kNegativeExtentDirection)
    
    Dim oExtrude1 As ExtrudeFeature
    Set oExtrude1 = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)
    
    Set oCircle = oSketch.SketchCircles.AddByCenterRadius(oTransGeom.CreatePoint2d(0.75, 0), 1)
    oPaths.Clear
    oPaths.Add oCircle
    
    Set oProfile = oSketch.Profiles.AddForSolid(False, oPaths)
    
    Set oExtrudeDef = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kNewBodyOperation)
    Call oExtrudeDef.SetDistanceExtent(1, kNegativeExtentDirection)
    
    Dim oExtrude2 As ExtrudeFeature
    Set oExtrude2 = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)
    
    Dim oTools As ObjectCollection
    Set oTools = ThisApplication.TransientObjects.CreateObjectCollection
    oTools.Add oExtrude2.SurfaceBodies.Item(1)
    
    Dim oCombine As CombineFeature
    Set oCombine = oCompDef.Features.CombineFeatures.Add(oExtrude1.SurfaceBodies.Item(1), oTools, kCutOperation, True)
    
    Dim oClientDef As ClientFeatureDefinition
    Set oClientDef = oCompDef.Features.ClientFeatures.CreateDefinition(, oExtrude1, oExtrude2)
    
    ' If we change the previous line to the next line, the ClientFeatures.Add method produces an error
    ' Set oClientDef = oCompDef.Features.ClientFeatures.CreateDefinition(, oExtrude1, oCombine)
    
    Dim oClient As ClientFeature
    Set oClient = oCompDef.Features.ClientFeatures.Add(oClientDef, "TestClientFeature1")
    
End Sub

I also tested it in C# and received a similar error:

It is interesting that we can create nested ClientFeatures including CombineFeature without error:

|__ ClientFeature

      |__ ClientFeature

      |__ CombineFeature

[SELT0001]

In the 2023 version of Inventor, the envelope feature is not needed. This is already required by later versions (2024 and 2025). I can add more. If the ClientFeature contains a Combine Feature in which the "Keep Toolbody" option is disabled, then something in the data of the modeled part is completely corrupted. It is not possible to proceed with any modeling of the part. Inventor hangs and doesn't even give any error message. Suppose you save the part file after creating such a Clientfeature, it is irreversibly damaged. In that case, it cannot be opened, and we receive the error message "Internal error in persistence operation".