Insert Thin Cut Extrude Example (C#)

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

//------------------------------------------------------
// Preconditions: Verify that the specified part exists.
//
// Postconditions:
// 1. Opens the part.
// 2. Inserts a thin cut extrude feature in the part.
// 3. Examine the FeatureManager design tree and
//    graphics area.
//
// NOTE: Because this part document is used elsewhere,
// do not save changes.
//-----------------------------------------------------
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:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2018\\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;

    }
}