Create Extrusion Feature Example (C#)

//----------------------------------------------------------------------------
// Preconditions: Verify that the specified part template exists.
//
// Postconditions:
// 1. Creates a Boss-Extrude1 feature.
// 2. Examine the FeatureManager design tree and graphics area.
// ---------------------------------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
namespace CreateExtrusionFeature_CSharp.csproj
{
    partial class SolidWorksMacro
    {

        Feature myFeature;
        ModelDoc2 Part;
        RefPlane myRefPlane;

        bool boolstatus;

        public void Main()
        {
            Part = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SOLIDWORKS\\SOLIDWORKS 2016\\templates\\Part.prtdot", 0, 0, 0);
            Part = (ModelDoc2)swApp.ActiveDoc;

            boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, true, 0, null, 0);
            myRefPlane = (RefPlane)Part.FeatureManager.InsertRefPlane(8, 0.01, 0, 0, 0, 0);
            boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, true, 0, null, 0);
            myRefPlane = (RefPlane)Part.FeatureManager.InsertRefPlane(8, 0.02, 0, 0, 0, 0);

            boolstatus = Part.Extension.SelectByID2("Plane2", "PLANE", 0, 0, 0, false, 0, null, 0);
            object vSkLines = null;
            vSkLines = Part.SketchManager.CreateCornerRectangle(-0.0250462141853123, 0.0157487558892494, 0, 0.0275128867944718, -0.015559011842391, 0);

            Part.SketchManager.InsertSketch(true);

            // Sketch to extrude
            boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, false, 0, null, 0);
            // Start condition reference
            boolstatus = Part.Extension.SelectByID2("Plane2", "PLANE", 0.00105020593408751, -0.00195369982668282, 0.0248175428318827, true, 32, null, 0);
            // End condition reference
            boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", 0.0068370744701368, -0.004419862088339, 0.018892268568016, true, 1, null, 0);

            // Boss extrusion start condition reference is Plane2, and the extrusion end is offset 3 mm from the end condition reference, Plane1
            myFeature = (Feature)Part.FeatureManager.FeatureExtrusion3(true, false, true, (int)swEndConditions_e.swEndCondOffsetFromSurface, 0, 0.003, 0.003, false, false, false,
            false, 0.0174532925199433, 0.0174532925199433, false, false, false, false, true, true, true,
            (int)swStartConditions_e.swStartSurface, 0, false);

        }

        public SldWorks swApp;

    }
}