Insert Thin Cut Extrude Example (C#)

This example shows how to insert a thin cut extrude feature.

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

// Preconditions: Specified part exists.

//

// Postconditions: A thin cut extrude feature in inserted in

// the part.

//

// NOTE: Because this 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 FeatureCutThin2FeatureManagerCSharp.csproj

 

{

    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 errorstatus = 0;

            int warnings = 0;

 

            // Open part

            swApp.OpenDoc6("C:\\Program Files\\SolidWorks Corp\\SolidWorks\\samples\\tutorial\\api\\water.sldprt", 1, 0, "", ref errorstatus, ref warnings);

            swModel = (ModelDoc2)swApp.ActiveDoc;

 

            // Select face on which to sketch a circle

            swModelDocExt = (ModelDocExtension)swModel.Extension;

            boolstatus = swModelDocExt.SelectByID2("", "FACE", 0.0001655362220845, -0.0477671348753, 0.072, false, 0, null, 0);

            swModel.ShowNamedView2("*Normal To", (int)swStandardViews_e.swBackView);

            swModel.ClearSelection2(true);

 

            // Sketch a circle

            swSketchManager = (SketchManager)swModel.SketchManager;

            swSketchSegment = (SketchSegment)swSketchManager.CreateCircle(0.0, 0.0, 0.0, 0.030255, -0.042492, 0.0);

            swModel.ClearSelection2(true);

 

            // Create the thin cut extrude

            boolstatus = swModelDocExt.SelectByID2("Arc1", "SKETCHSEGMENT", 0, 0, 0, false, 0, null, 0);

            swFeatureManager = (FeatureManager)swModel.FeatureManager;

            swFeature = (Feature)swFeatureManager.FeatureCutThin2(true, false, false, (int)swEndConditions_e.swEndCondBlind,

                (int)swEndConditions_e.swEndCondBlind, 0.01, 0.01, false, false, false,

                false, 0.01745329251994, 0.01745329251994, false, false, false, false, 0.01, 0.01, 0.01,

                0, 0, false, 0.005, true, true, (int)swStartConditions_e.swStartSketchPlane, 0, false);

            swModel.ShowNamedView2("*Isometric", (int)swStandardViews_e.swIsometricView);

 

        }

 

        /// <summary>

        /// The SldWorks swApp variable is pre-assigned for you.

        /// </summary>

        public SldWorks swApp;

 

    }

}