Hide Table of Contents

Insert New Virtual Component Example (C#)

This example shows how to insert a new part as a virtual component in an assembly and save it to an external file.

// Preconditions: 
// 1. Add a reference to Microsoft Scripting Runtime (right-click
//    the name of the project in the Project Explorer and click Add Reference >
//    the Browse tab > C:\windows\system32\scrrun.dll > OK.
// 2. Open public_documents\tutorial\smartcomponents\stepped_shaft.sldasm
// 3. Select a planar face on the assembly.
// 4. Open the Immediate window.
// 5. Step through this macro by pressing F8.
// Postconditions: 
// 1. Inserts a new part as a virtual component in the assembly. 
// 2. Attempts to save the virtual component to an external file, 
// 3. Examine the Immediate window and FeatureManager design tree.
// NOTE: Because this assembly is used elsewhere,
// do not save changes.
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System;
using System.Diagnostics;
using Scripting;
namespace Macro1CSharp.csproj
    partial class SolidWorksMacro
        ModelDoc2 swModel;
        AssemblyDoc swAssy;
        Component2 swComponent;
        SelectionMgr swSelMgr;
        FileSystemObject objFSO;
        string compName;
        object[] splits;
        long status;
        public void Main()
            swModel = (ModelDoc2)swApp.ActiveDoc;
            swAssy = (AssemblyDoc)swModel;
            // Get the pre-selected planar face 
            Face2 swFeature = default(Face2);
            swSelMgr = (SelectionMgr)swModel.SelectionManager;
            swFeature = (Face2)swSelMgr.GetSelectedObject6(1, 0);
            // Create the part and insert it as a virtual component 
            // in the assembly 
            status = swAssy.InsertNewVirtualPart(swFeature, out swComponent);
            if (status == 1)
                Debug.Print("Virtual component inserted!");
                Debug.Print("Name of virtual component: " + swComponent.Name2);
                // Check to see if the part is a virtual component 
                Debug.Print("Is component virtual? " + swComponent.IsVirtual);
                objFSO = new Scripting.FileSystemObject();
                splits = swComponent.Name2.Split('^');
                compName = objFSO.GetParentFolderName(swModel.GetPathName()) + "\\" + splits[0];
                ModelDoc2 compModel = default(ModelDoc2);
                compModel = (ModelDoc2)swComponent.GetModelDoc();
                if (compModel.GetType() == (int)swDocumentTypes_e.swDocPART)
                    compName = compName + ".sldprt";
                    compName = compName + ".sldasm";
                Debug.Print("Path and name of virtual component: " + compName);
                bool ret;
                ret = swComponent.SaveVirtualComponent(compName);
                if (ret)
                    Debug.Print("    Virtual component saved!");
                    Debug.Print("    Virtual component not saved!");
                    Debug.Print("       Check the folder's attributes where to save the virtual component and check your permissions to this folder.");
                Debug.Print("Error code returned when attempting to insert new part as virtual component: " + status);
        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

Subject:   Feedback on Help Topics
Page:   Insert New Virtual Component Example (C#)
*   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:


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

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.