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Insert Surface-cut Feature Example (C#)

This example shows how to insert a surface-cut feature.

// ******************************************************************************
// Preconditions: 
// 1. Specified file to open exists.
// 2. Open the Immediate window.
// Postconditions:
// 1. Opens part whose intersecting solid bodies to cut with a plane.
// 2. Creates a plane named Plane1.
// 3. Selects Plane1 to cut all intersecting solid bodies.
// 4. Inserts the surface-cut feature. All intersecting solid bodies
//    were cut by the plane.
// 5. Examine the graphics area and Immediate window to verify.
// NOTE: Because this part document is used elsewhere, do not
// save any changes when closing it.
// ******************************************************************************
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
using System.Diagnostics;
namespace InsertCutSurface2CSharp.csproj
    partial class SolidWorksMacro
        public void Main()
            PartDoc swPart = default(PartDoc);
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            Feature swFeature = default(Feature);
            FeatureManager swFeatureManager = default(FeatureManager);
            RefPlane swRefPlane = default(RefPlane);
            SurfCutFeatureData swSurfaceCutFeature = default(SurfCutFeatureData);
            bool status = false;
            string fileName = null;
            int errors = 0;
            int warnings = 0;
            // Open part to cut with a plane
            fileName = "C:\\Program Files\\SolidWorks Corp\\SolidWorks\\samples\\tutorial\\multibody\\multi_inter.sldprt";
            swPart = (PartDoc)swApp.OpenDoc6(fileName, (int)swDocumentTypes_e.swDocPART, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, ""ref errors, ref warnings);
            swModel = (ModelDoc2)swPart;
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            // Create and select the plane to cut the 
            // intersecting solid bodies in the part
            status = swModelDocExt.SelectByID2("Front""PLANE", 0, 0, 0, true, 0, null, 0);
            swFeatureManager = (FeatureManager)swModel.FeatureManager;
            swRefPlane = (RefPlane)swFeatureManager.InsertRefPlane((int)swRefPlaneReferenceConstraints_e.swRefPlaneReferenceConstraint_Distance, 0.045, 0, 0, 0, 0);
            status = swModelDocExt.SelectByID2("Plane1""PLANE", 0, 0, 0, true, 0, null, 0);
            // Insert surface-cut feature to cut 
            // all intersecting solid bodies
            swFeature = (Feature)swFeatureManager.InsertCutSurface(false, 0, falsetruenullout errors);
            Debug.Print("Were any errors generated by the surface cut (0 = no errors)? " + errors);
            // Get surface-cut feature and some properties
            swSurfaceCutFeature = (SurfCutFeatureData)swFeature.GetDefinition();
            Debug.Print("Name of surface-cut feature: " + swFeature.Name);
            Debug.Print(" Is feature scope on? " + swSurfaceCutFeature.FeatureScope);
            Debug.Print(" Number of bodies cut by the plane: " + swSurfaceCutFeature.GetFeatureScopeBodiesCount());
            Debug.Print(" Is auto-select on? " + swSurfaceCutFeature.AutoSelect);
        /// <summary>
        /// The SldWorks swApp variable is pre-assigned for you.
        /// </summary>
        public SldWorks swApp;

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