Hide Table of Contents

Create and Modify Move Face Feature Example (C#)

This example shows how to create a Move Face feature by translating a face on a part and then how to modify that Move Face feature.


// Preconditions:

// 1. The specified SolidWorks document exists

//    on your system.

// 2. Set a break point at the OpenDoc6 statement.

// 3. Step through (press F8) the macro.


// Postconditions: A Move Face feature is created and then

// modified.


// NOTE: Because the specified SolidWorks document is used by

//       a SolidWorks online tutorial, do not save any changes

//       when closing the document.


using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

using System;


namespace InsertMoveFace2FeatureManagerCSharp.csproj


    public partial class SolidWorksMacro


        public void Main()


            ModelDoc2 swModel = default(ModelDoc2);

            ModelDocExtension swModelDocExt = default(ModelDocExtension);

            FeatureManager swFeatMgr = default(FeatureManager);

            Feature swFeat = default(Feature);

            MoveFaceFeatureData swMoveFaceFeat = default(MoveFaceFeatureData);

            double[] transParams = null;

            bool boolstatus = false;

            double[] triadParams = new double[3];

            int fileerror = 0;

            int filewarning = 0;


            // Open the SolidWorks document

            swApp.OpenDoc6("C:\\Program Files\\SolidWorks Corp\\SolidWorks\\samples\\tutorial\\assemblymates\\knee.sldprt", (int)swDocumentTypes_e.swDocPART, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, "", ref fileerror, ref filewarning);


            swModel = (ModelDoc2)swApp.ActiveDoc;

            swModelDocExt = swModel.Extension;

            swFeatMgr = swModel.FeatureManager;


            // Translation parameters

            triadParams[0] = 0;

            triadParams[1] = 0.05;

            triadParams[2] = 0;

            transParams = triadParams;


            // Select face to move

            boolstatus = swModel.Extension.SelectByID2("", "FACE", 0.04239074672171, 0.01587499999999, 0.3283508339712, false, 1, null, 0);


            // Create the Move Face feature by

            // moving the selected face

            swFeat = (Feature)swFeatMgr.InsertMoveFace2(1, false, 0, 0, (transParams), null);


            // Modify the Move Face feature

            swMoveFaceFeat = (MoveFaceFeatureData)swFeat.GetDefinition();


            // Roll back the Move Face feature

            swMoveFaceFeat.AccessSelections(swModel, null);

            triadParams[0] = 0;

            triadParams[1] = 0.1;

            triadParams[2] = 0;

            transParams = triadParams;

            swMoveFaceFeat.TriadTranslationParameters = (transParams);


            // Roll back the part with the modified Move Face feature             

            swFeat.ModifyDefinition(swMoveFaceFeat, swModel, null);




        /// <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

Subject:   Feedback on Help Topics
Page:   Create and Modify Move Face Feature 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) 2012 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.