Change the Plane of a Sketch Example (C#)

//----------------------------------------------------------------------------
// Preconditions: Verify that the specified template exists.
//
// Postconditions:
// 1. Creates a new part document with a sketch of a spline.
// 2. Changes the plane of the sketch Top Plane to the Front Plane.
// 3. Examine the FeatureManager design tree and graphics area.
//----------------------------------------------------------------------------

	using Microsoft.VisualBasic;

	using System;

	using System.Collections;

	using System.Collections.Generic;

	using System.Data;

	using System.Diagnostics;

	using SolidWorks.Interop.sldworks;

	using SolidWorks.Interop.swconst;

	using System.Runtime.InteropServices;

	namespace ChangeSketchPlane_CSharp.csproj

	{

	    partial class SolidWorksMacro

	    {


	        ModelDoc2 Part;

	        SketchSegment skSegment;

	        bool boolstatus;


	        public void Main()

	        {

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


	            boolstatus = Part.Extension.SelectByID2("Top 
	Plane", "PLANE", -0.0494443883882606, 
	0.010829578664819, 0.0187336739521956, true, 
	0, null, 
	0);

	            Part.SketchManager.InsertSketch(true);


	            object pointArray = null;

	            double[] 
	points = new double[12];


	            points[0] = -0.0696700449874595;

	            points[1] = -0.0205096087491173;

	            points[2] = 0;

	            points[3] = -0.0349133034431539;

	            points[4] = 0.0151865041882777;

	            points[5] = 0;

	            points[6] = 0.0183177421652422;

	            points[7] = 0;

	            points[8] = 0;

	            points[9] = 0.060902578651959;

	            points[10] = 0.0336608082523681;

	            points[11] = 0;

	            pointArray = points;


	            skSegment = Part.SketchManager.CreateSpline((pointArray));

	            Part.SketchManager.InsertSketch(true);


	            boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 
	0, 0, 0, false, 
	0, null, 
	0);

	            boolstatus = Part.Extension.SelectByID2("Top 
	Plane", "PLANE", 0, 0, 0, true, 0, null, 0);

	            boolstatus = Part.DeSelectByID("Top Plane", "PLANE", 0, 0, 0);


	            // Select sketch and new plane 
	for the sketch

	            boolstatus = Part.Extension.SelectByID2("Front 
	Plane", "PLANE", 0, 0, 0, true, 0, null, 0);

	            boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 
	0, 0, 0, false, 
	0, null, 
	0);

	            // Change the plane of the 
	sketch

	            boolstatus = Part.Extension.ChangeSketchPlane(1, null);

	            boolstatus = Part.EditRebuild3();


	            Part.ShowNamedView2("*Isometric", 
	7);

	            boolstatus = Part.Extension.SelectByID2("Front 
	Plane", "PLANE", 0, 0, 0, true, 0, null, 0);


	        }


	        public SldWorks swApp;


	    }


	}