Hide Table of Contents

Create Shell Feature Example (C#)

This example shows how to create a shell feature.

//---------------------------------------------------------------------------
// Preconditions:
// 1. Verify that the specified model document exists.
// 2. Open an Immediate window.
//
// Postconditions:
// 1. Selects a face to remove from the model to create the shell.
// 2. Creates Shell1.
// 3. Inspect the Immediate window, graphics area, and
//    FeatureManager design tree.
//
// 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 CreateShellFeature_CSharp.csproj
{
    partial class SolidWorksMacro
    {
 
        ModelDoc2 swModel;
        SelectionMgr swSelMgr;
        SelectData swSelData;
        Feature swFeat;
        ShellFeatureData swShell;
        object[] vFaceRemArr;
        object vFaceRem;
        Face2 swFaceRem;
        object[] vMultiFaceArr;
        object vMultiFace;
        Face2 swMultiFace;
        Entity swEnt;
        int i;
        bool bRet;
        int longstatus;
        int longwarnings;
 
 
        public void Main()
{
swModel = (ModelDoc2)swApp.OpenDoc6("C:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2017\\tutorial\\api\\block20.sldprt", 1, 0, ""ref longstatus, ref longwarnings);
swApp.ActivateDoc2("block20"falseref longstatus);
swModel = (ModelDoc2)swApp.ActiveDoc;
 
bRet = swModel.Extension.SelectByID2("""FACE", -0.0150558029249623, 0.0396239999999466, -0.018063862472502, false, 1, null, 0);
swModel.InsertFeatureShell(0.00254, false);
 
swSelMgr = (SelectionMgr)swModel.SelectionManager;
swSelData = swSelMgr.CreateSelectData();
swFeat = (Feature)swSelMgr.GetSelectedObject6(1, -1);
swShell = (ShellFeatureData)swFeat.GetDefinition();
 
// Get shell data
Debug.Print("File = " + swModel.GetPathName());
Debug.Print("  " + swFeat.Name);
Debug.Print("    Direction: " + swShell.Direction);
Debug.Print("    Thickness: " + swShell.Thickness * 1000.0 + " mm");
Debug.Print("    Count of faces removed: " + swShell.FacesRemovedCount);
Debug.Print("    Count of faces with alternative thicknesses: " + swShell.GetMultipleThicknessFacesCount());
 
bRet = swShell.AccessSelections(swModel, null);
swModel.ClearSelection2(true);
 
vFaceRemArr = (object[])swShell.FacesRemoved;
 
for (i =0; i< vFaceRemArr.GetLength(0); i++) {
vFaceRem = vFaceRemArr[i];
swFaceRem = (Face2)vFaceRem;
swEnt = (Entity)swFaceRem;
 
bRet = swEnt.Select4(true, swSelData);
}
 
swModel.ClearSelection2(true);
vMultiFaceArr = (object[])swShell.MultipleThicknessFaces;
 
foreach (object vMultiFace_loopVariable in vMultiFaceArr) {
vMultiFace = vMultiFace_loopVariable;
swMultiFace = (Face2)vMultiFace;
swEnt = (Entity)swMultiFace;
 
Debug.Print("    Alternative thickness in mm at face (" + i + "): " + swShell.GetMultipleThicknessAtIndex(i) * 1000.0);
i = i + 1;
 
bRet = swEnt.Select4(true, swSelData);
}
 
swModel.ClearSelection2(true);
swShell.ReleaseSelectionAccess();
 
 
}
 
        /// <summary>
        /// The SldWorks swApp variable is pre-assigned for you.
        /// </summary>
 
        public SldWorks swApp;
 
    }
 
}



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Create Shell Feature Example (C#)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2017 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.