Public Sub SweepFeature()
' Set a reference to the currently active document.
' This assumes that it is a part document.
Dim oPartDoc As PartDocument
Set oPartDoc = ThisApplication.ActiveDocument
' Set a reference to the component definition.
Dim oCompDef As PartComponentDefinition
Set oCompDef = oPartDoc.ComponentDefinition
' Set a reference to the transient geometry object.
Dim oTG As TransientGeometry
Set oTG = ThisApplication.TransientGeometry
' Create some workpoints that will be used for the 3D sketch.
Dim oWPs(1 To 5) As WorkPoint
Set oWPs(1) = oCompDef.WorkPoints.AddFixed(oTG.CreatePoint(0, 0, 0))
Set oWPs(2) = oCompDef.WorkPoints.AddFixed(oTG.CreatePoint(3, 0, 0))
Set oWPs(3) = oCompDef.WorkPoints.AddFixed(oTG.CreatePoint(3, 4, 0))
Set oWPs(4) = oCompDef.WorkPoints.AddFixed(oTG.CreatePoint(3, 4, 2))
Set oWPs(5) = oCompDef.WorkPoints.AddFixed(oTG.CreatePoint(6, 4, 2))
' Create a new 3D Sketch.
Dim oSketch3D As Sketch3D
Set oSketch3D = oPartDoc.ComponentDefinition.Sketches3D.Add
' Draw 3D lines. The first line is drawn between two of the work points.
Dim oLine As SketchLine3D
Set oLine = oSketch3D.SketchLines3D.AddByTwoPoints(oWPs(1), oWPs(2), True, 1)
' This second and subsequent lines are drawn between a 3D sketch point and a work point.
' The work point is obtained from the previous line. Because the two lines will share
' this 3D sketch point, Inventor will treat them as connected lines when creating any
' paths.
Set oLine = oSketch3D.SketchLines3D.AddByTwoPoints(oLine.EndPoint, oWPs(3), True, 1)
Set oLine = oSketch3D.SketchLines3D.AddByTwoPoints(oLine.EndPoint, oWPs(4), True, 0.75)
Set oLine = oSketch3D.SketchLines3D.AddByTwoPoints(oLine.EndPoint, oWPs(5), True, 1)
' Create a 2D sketch.
Dim oSketch As PlanarSketch
Set oSketch = oCompDef.Sketches.Add(oCompDef.WorkPlanes.Item(2))
' Determine the model origin relative to the sketch space.
Dim oOrigin As Point2d
Set oOrigin = oSketch.ModelToSketchSpace(oTG.CreatePoint(0, 0, 0))
' Create two lines.
Dim oNewPoint As Point2d
Set oNewPoint = oTG.CreatePoint2d(oOrigin.X, oOrigin.Y - 4)
Dim oSketchLine1 As SketchLine
Set oSketchLine1 = oSketch.SketchLines.AddByTwoPoints(oOrigin, oNewPoint)
oNewPoint.X = oNewPoint.X + 3
Dim oSketchLine2 As SketchLine
Set oSketchLine2 = oSketch.SketchLines.AddByTwoPoints(oSketchLine1.EndSketchPoint, oNewPoint)
' Create a fillet between the two lines.
Call oSketch.SketchArcs.AddByFillet(oSketchLine1, oSketchLine2, 1, oSketchLine1.StartSketchPoint.Geometry, oSketchLine2.EndSketchPoint.Geometry)
' Get the end of the 2d sketch in model space.
Dim oModelPoint As Point
Set oModelPoint = oSketch.SketchToModelSpace(oSketchLine2.EndSketchPoint.Geometry)
' Create a work plane at the end of the 2D sketch.
Dim oWP As WorkPlane
Set oWP = oCompDef.WorkPlanes.AddByNormalToCurve(oSketchLine2, oSketchLine2.EndSketchPoint)
' Create a path. Because the 3D and 2D sketches physically connect the path will include
' both of them.
Dim oPath As Path
Set oPath = oCompDef.Features.CreatePath(oSketchLine2)
' Create a sketch containing a circle.
Set oSketch = oCompDef.Sketches.Add(oWP)
Set oOrigin = oSketch.ModelToSketchSpace(oTG.CreatePoint(0, 0, 0))
Call oSketch.SketchCircles.AddByCenterRadius(oSketch.ModelToSketchSpace(oModelPoint), 0.375)
' Create a profile.
Dim oProfile As Profile
Set oProfile = oSketch.Profiles.AddForSolid
' Create the sweep feature.
Dim oSweep As SweepFeature
Set oSweep = oCompDef.Features.SweepFeatures.AddUsingPath(oProfile, oPath, kJoinOperation)
End Sub
