Create Hole Wizard Hole Example (C#)

This example shows how to create a hole using the hole wizard.

//--------------------------------- ---------------------------
// Preconditions: Verify that the part template exists. 
// 
// Postconditions: 
// 1. Creates a part.
// 2. Inserts a hole in the part using the hole wizard.
// 3. Examine the graphics area and FeatureManager design tree.
//-------------------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System;

namespace Macro1CSharp.csproj
{

    partial class SolidWorksMacro
    {
        public void Main()
        {

            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            FeatureManager swFeatMgr = default(FeatureManager);
            Feature swFeat = default(Feature);
            SketchManager swSketchMgr = default(SketchManager);
            object sketchLines = null;
            int status = 0;
            bool boolstatus = false;
            double[] P1 = new double[3];
            double[] P2 = new double[3];
            double[] P3 = new double[3];

            // Create the model for the wizard hole 
            swApp.ResetUntitledCount(0, 0, 0);
            swModel = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SOLIDWORKS\\SOLIDWORKS 2016\\templates\\Part.prtdot", 0, 0, 0);
            swApp.ActivateDoc2("Part1", false, ref status);
            swModel = (ModelDoc2)swApp.ActiveDoc;
            swSketchMgr = swModel.SketchManager;
            swModelDocExt = swModel.Extension;
            swFeatMgr = swModel.FeatureManager;
            sketchLines = swSketchMgr.CreateCornerRectangle(-0.05096498314664, 0.05060941349678, 0, 0.1021670127265, -0.05037236706354, 0);
            boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, false, 0, null, 0);
            boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            swFeat = swFeatMgr.FeatureExtrusion2(true, false, false, 0, 0, 0.381, 0.381, false, false, false, false, 0.01745329251994, 0.01745329251994, false, false, false, false, true, true, true, 0, 0, false);

            //Create three points for the reference plane 
            P1[0] = -0.0141556764402858;
            P1[1] = 0.00194061273859598;
            P1[2] = 0;
            P2[0] = -0.0141556764402858;
            P2[1] = 0.00194061273859598;
            P2[2] = 1;
            P3[0] = -0.149976101832345;
            P3[1] = -0.988792859011662;
            P3[2] = 0;

            //Create the reference plane 
            swModel.CreatePlaneFixed2(P1, P2, P3, false);

            //Select reference plane 
            boolstatus = swModelDocExt.SelectByID2("Plane1", "PLANE", -0.0156784487003801, -0.00916715285390111, 0.0558270998665543, false, 0, null, 0);

            // Create the hole wizard hole 
            swFeat = swFeatMgr.HoleWizard5((int)swWzdGeneralHoleTypes_e.swWzdCounterSink, (int)swWzdHoleStandards_e.swStandardAnsiMetric, (int)swWzdHoleStandardFastenerTypes_e.swStandardAnsiMetricFlatHead82, "M2", (int)swEndConditions_e.swEndCondThroughAll, 0.0102, 0.010312189893273, 0, 0.0044, 1.57079632679489, 0.000152189893272978, 0, 2.05948851735331, 0, 0, 0, 1, 0, 0, 0, "", false, true, true, true, true, false);

        }

        public SldWorks swApp;

    }

}