Insert Cut Extrude Example (C#)

This example shows how to insert a cut extrude feature.

//----------------------------------------------------------
// Preconditions: Verify that specified part to open exists.
//
// Postconditions:
// 1. Inserts a cut extrude feature is in the model.
// 2. Examine the graphics area.
//
// NOTE: Because the part document is used elsewhere, do not save
// changes.
//----------------------------------------------

using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System;

namespace FeatureCut3FeatureManagerCSharp.csproj

{

    public partial class SolidWorksMacro

    {

        public void Main()

        {

            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            SketchManager swSketchManager = default(SketchManager);
            SketchSegment swSketchSegment = default(SketchSegment);
            FeatureManager swFeatureManager = default(FeatureManager);
            Feature swFeature = default(Feature);
            bool boolstatus = false;
            int fileerror = 0;
            int filewarning = 0;

            // Open part document
            swApp.OpenDoc6("C:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2018\\samples\\tutorial\\api\\plate.sldprt", (int)swDocumentTypes_e.swDocPART, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, "", ref fileerror, ref filewarning);
            swModel = (ModelDoc2)swApp.ActiveDoc;
            swModelDocExt = (ModelDocExtension)swModel.Extension;
 

            // Select the face where to sketch a circle
            boolstatus = swModelDocExt.SelectByID2("", "FACE", -0.02031412853728, 0.006977746007294, -0.008053400767039, false, 0, null, 0);
            swSketchManager = (SketchManager)swModel.SketchManager;
            swSketchManager.InsertSketch(true);
            swModel.ClearSelection2(true);
 

            // Sketch a circle
            swSketchSegment = (SketchSegment)swSketchManager.CreateCircle(0.0, 0.0, 0.0, 0.01708, -0.030458, 0.0);
            boolstatus = swModelDocExt.SelectByID2("Arc1", "SKETCHSEGMENT", 0, 0, 0, false, 0, null, 0);
            swModel.ClearSelection2(true);
 

            // Insert a cut-extrude feature using the circle
            swFeatureManager = (FeatureManager)swModel.FeatureManager;
swFeature = (Feature)swFeatureManager.FeatureCut3(true, false, false, (int)swEndConditions_e.swEndCondThroughAll,
  (int)swEndConditions_e.swEndCondBlind, 0.01, 0.01, false, false, false,
               false, 0.01745329251994, 0.01745329251994, false, false, false, false, false, true, true,
               false, false, false, (int)swStartConditions_e.swStartSketchPlane, 0, false);
        }

        /// <summary>
        /// The SldWorks swApp variable is pre-assigned for you.
        /// </summary>
        public SldWorks swApp;

    }

}