Insert Cut Extrude Example (C#)

This example shows how to insert a cut extrude feature.

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

// Preconditions: Specified file exists.

//

// Postconditions: A cut extrude feature is inserted in

// the model.

//

// NOTE: Because the part document is used by an online

// SOLIDWORKS tutorial, do not save any changes when

// closing the document.

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

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:\\Program Files\\SOLIDWORKS Corp\\SOLIDWORKS\\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;

 

    }

}