Replace Sketch Entity Example (C#)

//----------------------------------------------------------------------------
// Preconditions: Verify that the specified template exists.
//
// Postconditions:
// 1. Opens a new part and creates Boss-Extrude1.
// 2. Replaces a sketch line with a sketch arc and modifies
//    Boss-Extrude1.
// 3. Examine the graphics area.
// ---------------------------------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
namespace ReplaceSketch_CSharp.csproj
{
    partial class SolidWorksMacro
    {

        ModelDoc2 Part;
        Feature myFeature;
        SketchSegment skSegment;

        bool boolstatus;

        public void Main()
        {
            Part = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SOLIDWORKS\\SOLIDWORKS 2017\\templates\\Part.prtdot", 0, 0, 0);
            Part = (ModelDoc2)swApp.ActiveDoc;

            boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -0.048646278525398, 0.0222864804840025, 0.0105288722478765, false, 0, null, 0);
           
            object vSkLines = null;
            vSkLines = Part.SketchManager.CreateCornerRectangle(-0.0338155129850894, 0.0167825138518592, 0, 0.0551067619016271, -0.0245475575743612, 0);
            Part.ClearSelection2(true);
            Part.SketchManager.InsertSketch(true);
            Part.ShowNamedView2("*Trimetric", 8);
           
            boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, false, 4, null, 0);

            myFeature = Part.FeatureManager.FeatureExtrusion2(true, false, false, 0, 0, 0.01778, 0.00254, false, false, false,
            false, 0.0174532925199433, 0.0174532925199433, false, false, false, false, true, true, true,
            0, 0, false);
          
            boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, false, 0, null, 0);
            Part.EditSketch();
            Part.ClearSelection2(true);

            skSegment = Part.SketchManager.Create3PointArc(-0.033816, 0.016783, 0.0, 0.055107, 0.016783, 0.0, 0.016009, 0.025458, 0.0);
            Part.ClearSelection2(true);

            boolstatus = Part.Extension.SelectByID2("Line1", "SKETCHSEGMENT", 0.00202904300411839, 0.0119654152286464, -0.00709549576220667, true, 0, null, 0);
            boolstatus = Part.Extension.SelectByID2("Arc1", "SKETCHSEGMENT", 0.00588878331207997, 0.0171023327681304, -0.0126221740799126, true, 0, null, 0);
            boolstatus = Part.SketchManager.SketchReplace(true);
         
            Part.SketchManager.InsertSketch(true);

        }


        public SldWorks swApp;

    }


}