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

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

//--------------------------------------------------------------------------

// Preconditions:

// 1. Open SolidWorks.

// 2. Verify the location of the part template.

//

// Postconditions:

// 1. Click the green check mark in the Modify dimension dialog

//   (look for the hidden dialog behind your other windows).

// 2. 3DSketch1 is in edit mode and contains a spline and a corner rectangle.

// 3. The display dimension of 63.238 mm appears on the y axis starting at

//    (-0.1, 0, 0.01111142101618) while the sketch is in edit mode.

//---------------------------------------------------------------------------

using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

using System;

namespace AddAlongYDimension_CSharp.csproj

{

    partial class SolidWorksMacro

    {

        ModelDoc2 Part;

        DisplayDimension myDisplayDim;

        bool boolstatus;

        int longstatus;

        public void Main()

        {

            swApp.ResetUntitledCount(0, 0, 0);

            Part = (ModelDoc2)swApp.NewDocument("C:\\Documents and Settings\\All Users\\Application Data\\SolidWorks\\SolidWorks 2010\\templates\\Part.prtdot", 0, 0, 0);

            swApp.ActivateDoc2("Part1", false, ref longstatus);

            Part = (ModelDoc2)swApp.ActiveDoc;

            Part.SketchManager.Insert3DSketch(true);

            object vSkLines = null;

            vSkLines = 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 = points;

            SketchSegment skSegment = default(SketchSegment);

            skSegment = 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 = Part.SketchManager.AddAlongYDimension(-0.1, 0, 0.01111142101618);

            Part.ClearSelection2(true);

            Part.ViewZoomtofit2();

        }

        public SldWorks swApp;

    }

}



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