Error occurs using SketchLines for a profile when trying to create an extrusion

Issue

I create a sketch to create an extrusion. An error is occurring when using the sketch to create a profile. The error occurs on this line. Why am I getting the error?

Set oProfile1 = tySketch.Profiles.AddForSolid"

Here is the VBA code I am using:

Sub Test()
    Dim App As Inventor.Application
    Set App = ThisApplication
    ' this code will only work on an active part
    Dim Part1 As PartDocument
    Set Part1 = ThisApplication.ActiveDocument
    Dim TG As TransientGeometry
    Set TG = App.TransientGeometry
   
    'try to read face with transient id 1
    Dim oFace As Face
    Set oFace = Part1.ComponentDefinition.SurfaceBodies(1).BindTransientKeyToObject(1)
   
    Dim tySketch As PlanarSketch
    Dim oWorkPlane As WorkPlane
    Set oWorkPlane = Part1.ComponentDefinition.WorkPlanes.AddFixed(TG.CreatePoint
    (oFace.Evaluator.RangeBox.MinPoint.X, 0, 0), TG.CreateUnitVector(0, 1, 0), TG.CreateUnitVector(0, 0, 1),
    False)
   
    Set oPartCompDef = Part1.ComponentDefinition
    Set tySketch = oPartCompDef.Sketches.Add(oWorkPlane)
   
    ' create some temporary variables for drawing lines
    Dim tyStartPoint As Point2d
    Dim tyEndPoint As Point2d
    Dim tyTmpPoint As Point2d
    Dim tyLine As SketchLine
    Set tyStartPoint = TG.CreatePoint2d(0, 0)
    Set tyEndPoint = TG.CreatePoint2d(0, 0)
    Set tyTmpPoint = TG.CreatePoint2d(0, 0)
   
    'draw some lines to create a shap fo the extrusion
    Set tyStartPoint = tySketch.ModelToSketchSpace(oFace.Evaluator.RangeBox.MinPoint)
    Set tyEndPoint = tySketch.ModelToSketchSpace(oFace.Evaluator.RangeBox.MaxPoint)
    tyTmpPoint.X = tyStartPoint.X
    tyTmpPoint.Y = tyEndPoint.Y
    Set tyLine = tySketch.SketchLines.AddByTwoPoints(tyStartPoint, tyTmpPoint)
    Set tyLine = tySketch.SketchLines.AddByTwoPoints(tyTmpPoint, tyEndPoint)
    Set tyLine = tySketch.SketchLines.AddByTwoPoints(tyEndPoint, tyStartPoint)
   
    ' try to create a profile
    Dim oProfile1 As Profile
    Set oProfile1 = tySketch.Profiles.AddForSolid
    ' Do an extrusion on the solid
    oExtrusion = oPartCompDef.Features.ExtrudeFeatures.AddByDistanceExtent(oProfile, 3, kSymmetricExtentDirection, kJoinOperation, Null)

End Sub

Solution

The error occurs because there are no constraints between the SketchLines. You can use SketchPoint.Merge to add the constraints.  You can also use a SketchPoint directly as an argument when the Sketch geometry is being created.

Set oFirstline = tySketch.SketchLines.AddByTwoPoints(¡¬¡¬)
        Set oSecondLine = tySketch.SketchLines.AddByTwoPoints(¡¬¡¬)
        Set oLastline = tySketch.SketchLines.AddByTwoPoints(¡¬¡¬)
 
        Call oFirstline.EndSketchPoint.Merge(
             oSecondLine.StartSketchPoint)
        Call oSecondLine.EndSketchPoint.Merge(
             oLastline.StartSketchPoint)
        Call oFirstline.StartSketchPoint.Merge(
             oLastline.EndSketchPoint)

Here is a VB.NET example that creates a sketch, uses SketchPoint.Merge and then creates an extrusion. Before running this code create a part with rectangular faces like a box. This example is from a button on a form in a standalone exe that connects to Inventor from out of process.

Imports Inventor
    Public Class Form1
        Dim m_inventorApp As Inventor.Application = Nothing
 
 
        Private Sub Button1_Click(ByVal sender As System.Object,
                ByVal e As System.EventArgs) Handles Button1.Click
            Try ' Try to get an active instance of Inventor
 
                Try
                    m_inventorApp = System.Runtime.InteropServices.
                     Marshal.GetActiveObject("Inventor.Application")
 
                Catch ' If not active, create a new Inventor session
 
                    Dim inventorAppType As Type = System.Type.
                           GetTypeFromProgID("Inventor.Application")
 
                    m_inventorApp = System.Activator.CreateInstance(
                                                    inventorAppType)
 
                    'Must be set visible explicitly
                    m_inventorApp.Visible = True
 
                End Try
 
            Catch
                System.Windows.Forms.MessageBox.Show(
                   "Error: couldn't create Inventor instance")
            End Try
 
            Test()
 
        End Sub
 
        Sub Test()
            Try
                ' this code will only work on an active part 
                Dim Part1 As PartDocument
                Part1 = m_inventorApp.ActiveDocument
 
                Dim TG As TransientGeometry
                TG = m_inventorApp.TransientGeometry
 
                'try to read face with transient id 1 
                Dim oFace As Face
                oFace = Part1.ComponentDefinition.
                   SurfaceBodies(1).BindTransientKeyToObject(1)
 
                Dim tySketch As PlanarSketch
                Dim oWorkPlane As WorkPlane
                oWorkPlane = Part1.ComponentDefinition.WorkPlanes.
                                        AddFixed(TG.CreatePoint _
                     (oFace.Evaluator.RangeBox.MinPoint.X, 0, 0),
                                  TG.CreateUnitVector(0, 1, 0), _
                     TG.CreateUnitVector(0, 0, 1), False)
 
                Dim oPartCompDef As PartComponentDefinition
                oPartCompDef = Part1.ComponentDefinition
                tySketch = oPartCompDef.Sketches.Add(oWorkPlane)
 
                'draw some lines to create a shape for the extrusion 
                Dim MinPoint As Point2d = tySketch.
                    ModelToSketchSpace(
                                  oFace.Evaluator.RangeBox.MinPoint)
                Dim MaxPoint As Point2d = tySketch.
                    ModelToSketchSpace(
                                  oFace.Evaluator.RangeBox.MaxPoint)
 
                Dim Pnt2 As Point2d = TG.CreatePoint2d(
                                             MaxPoint.X, MinPoint.Y)
 
                Dim tyLine1 As SketchLine = tySketch.SketchLines.
                                      AddByTwoPoints(MinPoint, Pnt2)
                Dim tyLine2 As SketchLine = tySketch.SketchLines.
                                      AddByTwoPoints(Pnt2, MaxPoint)
                tyLine1.EndSketchPoint.Merge(
                                           tyLine2.StartSketchPoint)
 
                Dim Pnt3 As Point2d = TG.CreatePoint2d(M
                                              inPoint.X, MaxPoint.Y)
 
                Dim tyLine3 As SketchLine = tySketch.SketchLines.
                                      AddByTwoPoints(MaxPoint, Pnt3)
                tyLine2.EndSketchPoint.Merge(
                                           tyLine3.StartSketchPoint)
 
                Dim tyLine4 As SketchLine = tySketch.SketchLines.
                                      AddByTwoPoints(Pnt3, MinPoint)
                tyLine3.EndSketchPoint.Merge(
                                           tyLine4.StartSketchPoint)
                tyLine4.EndSketchPoint.Merge(
                                           tyLine1.StartSketchPoint)
 
                ' try to create a profile 
                Dim oProfile1 As Profile
                oProfile1 = tySketch.Profiles.AddForSolid
 
                ' Do an extrusion on the solid
                Dim oExtrusion As ExtrudeFeature
                oExtrusion = oPartCompDef.Features.ExtrudeFeatures.
                                  AddByDistanceExtent(oProfile1, 3, _
          PartFeatureExtentDirectionEnum.kSymmetricExtentDirection, _
                    PartFeatureOperationEnum.kJoinOperation, Nothing)
            Catch ex As Exception
                MsgBox(ex.ToString())
            End Try
        End Sub
    End Class