Create Replace Face Feature Example (C#)

This example shows how to create a Replace Face feature.

//----------------------------------------------------------------------------
// Preconditions:
// 1. Verify that the specified model document exists.
// 2. Open an Immediate window.
//
// Postconditions:
// 1. Opens the specified part.
// 2. Creates Plane1, Surface-Extrude1, and Replace Face1.
// 3. Inspect the FeatureManager design tree, the graphics area, and the
//    Immediate window.
//
// NOTE: Because the model is used elsewhere, do not save changes.
// ---------------------------------------------------------------------------
using Microsoft.VisualBasic;
using System;
using System.Collections;
using System.Collections.Generic;
using System.Data;
using System.Diagnostics;
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
namespace ReplaceFace_CSharp.csproj
{
    partial class SolidWorksMacro
    {
 
 
        SelectionMgr selMgr;
        ModelDoc2 Part;
        Feature feat;
        ReplaceFaceFeatureData featData;
        bool boolstatus;
        int longstatus;
        int longwarnings;
 
 
        public void Main()
        {
 
            Part = swApp.OpenDoc6("C:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2018\\samples\\tutorial\\api\\block20.sldprt", 1, 0, "", ref longstatus, ref longwarnings);
            swApp.ActivateDoc2("block20", false, ref longstatus);
            Part = (ModelDoc2)swApp.ActiveDoc;
 
            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.00687152192142548, 0.0256655537640995, 0.049345602378537, true, 0, null, 0);
            RefPlane myRefPlane = default(RefPlane);
            myRefPlane = (RefPlane)Part.FeatureManager.InsertRefPlane(264, 0.05842, 0, 0, 0, 0);
            Part.ClearSelection2(true);
 
            object pointArray = null;
            double[] points = new double[15];
            points[0] = -0.0700496017443584;
            points[1] = 0.0582762055241233;
            points[2] = 0;
            points[3] = -0.0357558994484748;
            points[4] = 0.0853945497913173;
            points[5] = 0;
            points[6] = -0.00588719099721402;
            points[7] = 0.0671372129016845;
            points[8] = 0;
            points[9] = 0.0273002628375139;
            points[10] = 0.0878577815467452;
            points[11] = 0;
            points[12] = 0.0737626982062238;
            points[13] = 0.0582762055241233;
            points[14] = 0;
            pointArray = points;
            SketchSegment skSegment = default(SketchSegment);
            skSegment = Part.SketchManager.CreateSpline((pointArray));
            Part.SketchManager.InsertSketch(true);
            boolstatus = Part.Extension.SelectByID2("Spline1@Sketch2", "EXTSKETCHSEGMENT", -0.0549544681183813, 0.0875052976097064, 0, false, 0, null, 0);
            Part.ClearSelection2(true);
            boolstatus = Part.Extension.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, false, 4, null, 0);
            ((SelectionMgr)Part.SelectionManager).EnableContourSelection = true;
            boolstatus = Part.Extension.SelectByID2("Sketch2", "SKETCHCONTOUR", 0, 0, 0, true, 4, null, 0);
            Part.FeatureExtruRefSurface2(true, false, false, 0, 0, 0.14478, 0.14478, false, false, false,
            false, 0.0174532925199433, 0.0174532925199433, false, false, false, false);
            ((SelectionMgr)Part.SelectionManager).EnableContourSelection = false;
            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.0585444908073214, 0.0396239999998329, -0.0518899759430838, true, 0, null, 0);
            boolstatus = Part.Extension.SelectByID2("Surface-Extrude1", "SURFACEBODY", -0.0189730427370591, 0.0726880897401543, 0.115671174990496, true, 0, null, 0);
            Part.ClearSelection2(true);
            boolstatus = Part.Extension.SelectByID2("Surface-Extrude1", "BODYFEATURE", 0, 0, 0, false, 0, null, 0);
            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.0585444908073214, 0.0396239999998329, -0.0518899759430838, true, 1, null, 0);
            boolstatus = Part.Extension.SelectByID2("Surface-Extrude1", "SURFACEBODY", -0.0189730427370591, 0.0726880897401543, 0.115671174990496, true, 2, null, 0);
            Part.InsertFeatureReplaceFace();
            boolstatus = Part.Extension.SelectByID2("", "FACE", -0.0362064915135534, 0.0856902732399476, 0.127037337239983, false, 0, null, 0);
            Part.FeatureManager.HideBodies();
            boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", -0.0693294107213475, 0.0872697709380442, -0.0300713252946179, false, 0, null, 0);
            Part.BlankRefGeom();
 
            boolstatus = Part.Extension.SelectByID2("Replace Face1", "BODYFEATURE", 0, 0, 0, false, 0, null, 0);
            selMgr = (SelectionMgr)Part.SelectionManager;
            feat = (Feature)selMgr.GetSelectedObject6(1, -1);
            featData = (ReplaceFaceFeatureData)feat.GetDefinition();
 
            featData.AccessSelections(Part, null);
 
            object[] vFacesToReplace = null;
            vFacesToReplace = (object[])featData.FacesForReplacement;
            Debug.Print(featData.GetFacesForReplacementCount() + " face replaced in " + ((Feature)((Face2)vFacesToReplace[0]).GetFeature()).Name);
            Debug.Print(featData.GetReplacementSurfacesCount() + " replacement surface ");
 
            featData.ReleaseSelectionAccess();
 
        }
 
 
 
        /// <summary>
        /// The SldWorks swApp variable is pre-assigned for you.
        /// </summary>
 
        public SldWorks swApp;
 
    }
}