Add Along X Dimension to 3D Sketch Example (C#)

This example shows how to add a display dimension along the x axis in a 3D sketch.

//----------------------------------------------------------------------------
// Preconditions: Verify that the specified part template exists.
//
// Postconditions:
// 1. Opens a new part document.
// 2. Inserts a 3D sketch.
// 3. Click the green check mark in the Modify dimension dialog
//    (If you don't see the dialog, look for it behind other open windows).
// 4. Puts 3DSketch1 in edit mode; 3DSketch1 contains a spline and a
//    corner rectangle.
// 5. Displays the display dimension of 84.46 mm on the x axis while the
//    sketch is in edit mode.
// 6. Examine the graphics area.
//----------------------------------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
 
namespace Macro1CSharp.csproj
{
    public partial class SolidWorksMacro
    {
 
        public void Main()
        {
            ModelDoc2 Part = default(ModelDoc2);
            DisplayDimension myDisplayDim = default(DisplayDimension);
            bool boolstatus = false;
            int longstatus = 0;
 
            longstatus = swApp.ResetUntitledCount(0, 0, 0);
            Part = (ModelDoc2)swApp.NewDocument("C:\\Documents and Settings\\All Users\\Application Data\\SOLIDWORKS\\SOLIDWORKS 2015\\templates\\Part.prtdot", 0, 0, 0);
            swApp.ActivateDoc2("Part1", false, ref longstatus);
            Part = (ModelDoc2)swApp.ActiveDoc;
 
            Part.SketchManager.Insert3DSketch(true);
            object vSkLines = null;
            vSkLines = (object)Part.SketchManager.CreateCornerRectangle(-0.05171778666374, 0.01933785938058, 0.03, 0.08445537697179, -0.04142795937025, -0.03);
            boolstatus = Part.Extension.SelectByID2("Right Plane", "PLANE", 0, 0, 0, false, 0, null, 0);
            Part.ClearSelection2(true);
 
            object pointArray = null;
            double[] points = new double[12];
            points[0] = 0;
            points[1] = -0.03591009660795;
            points[2] = 0.04608246573503;
            points[3] = 0;
            points[4] = 0.0147420284178;
            points[5] = 0.005170989573514;
            points[6] = 0;
            points[7] = -0.006478053228363;
            points[8] = -0.04282131900055;
            points[9] = 0;
            points[10] = -0.02294509596464;
            points[11] = -0.09396066420243;
            pointArray = (object)points;
 
            SketchSegment skSegment = default(SketchSegment);
            skSegment = (SketchSegment)Part.SketchManager.CreateSpline2((pointArray), true);
            Part.SketchManager.InsertSketch(true);
 
            boolstatus = Part.Extension.SelectByID2("3DSketch1", "SKETCH", 0, 0, 0, false, 0, null, 0);
            Part.EditSketch();
            boolstatus = Part.Extension.SelectByID2("Point5", "SKETCHPOINT", 0, -0.03591009660795, 0.04608246573503, false, 0, null, 0);
            boolstatus = Part.Extension.SelectByID2("Point4", "SKETCHPOINT", 0.08445537697179, 0.02732744880518, -0.01872625210654, true, 0, null, 0);
            myDisplayDim = (DisplayDimension)Part.SketchManager.AddAlongXDimension(0.05, -0.091, 0.001);
            Part.ClearSelection2(true);
 
            Part.ViewZoomtofit2();
 
        }
 
        /// <summary>
        ///  The SldWorks swApp variable is pre-assigned for you.
        /// </summary>
        public SldWorks swApp;
    }
}