Hide Table of Contents

Create Temporary Extruded Body Example (C#)

This example shows how to create a temporary extruded body.

//------------------------------------------------
// Preconditions: 
// 1. Verify that the specified part document 
//    template exists.
// 2. Add a reference to Microsoft.VisualBasic (right-click
//    the name of the project in the Project Explorer, click
//    Add Reference > the .NET tab > Microsoft.VisualBasic >
//    OK.
//
// Postconditions.
// 1. Opens a new part document.
// 2. Creates and selects a sheet (also called a surface) body.
// 3. Creates a temporary extruded body.
// 4. Examine the graphics area.
//------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
using Microsoft.VisualBasic;
 
namespace Macro1CSharp.csproj
{
    public partial class SolidWorksMacro
    {
 
 
        public void Main()
        {
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            FeatureManager swFeatureManager = default(FeatureManager);
            SketchManager swSketchManager = default(SketchManager);
            SelectionMgr swSelectionManager = default(SelectionMgr);
            SketchSegment sketchSegment = default(SketchSegment);
            Modeler swModeler = default(Modeler);
            MathUtility swMath = default(MathUtility);
            Body2 profileBody = default(Body2);
            Body2 extrudedBody = default(Body2);
            MathVector dirVector = default(MathVector);
            Surface planeSurf = default(Surface);
            Curve[] trimCurves = new Curve[4];
            double[] points = new double[12];
            object pointArray = null;
            double halfWidth = 0;
            double halfLength = 0;
            double[] startArr = new double[3];
            double[] endArr = new double[3];
            double[] ptArr = new double[3];
            double[] dirArr = new double[3];
            double slotWidth = 0;
            double slotLength = 0;
            double slotDepth = 0;
            bool slotThruAll = false;
            bool status = false;
 
            swModeler = (Modeler)swApp.GetModeler();
            swMath = (MathUtility)swApp.GetMathUtility();
            swModel = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SolidWorks\\SolidWorks 2014\\templates\\Part.prtdot", 0, 0, 0);
            swFeatureManager = (FeatureManager)swModel.FeatureManager;
            swSketchManager = (SketchManager)swModel.SketchManager;
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            swSelectionManager = (SelectionMgr)swModel.SelectionManager;
 
            //Create and select extruded surface body
            points[0] = -0.0720746414289124;
            points[1] = -0.0283600245263074;
            points[2] = 0;
            points[3] = -0.0514715593755;
            points[4] = -0.00345025084396866;
            points[5] = 0;
            points[6] = 0;
            points[7] = 0;
            points[8] = 0;
            points[9] = 0.0872558597840225;
            points[10] = 0.0521037067517796;
            points[11] = 0;
            pointArray = points;
            sketchSegment = (SketchSegment)swSketchManager.CreateSpline((pointArray));
            swSketchManager.InsertSketch(true);
            swModel.ClearSelection2(true);
            status = swModelDocExt.SelectByID2("Sketch1""SKETCH", 0, 0, 0, false, 4, null, 0);
            swFeatureManager.FeatureExtruRefSurface2(truefalsefalse, 0, 0, 0.0508, 0.00254, falsefalsefalse,
            false, 0.0174532925199433, 0.0174532925199433, falsefalsefalsefalsefalsefalsefalse,
            false);
            swSelectionManager.EnableContourSelection = false;
            status = swModelDocExt.SelectByID2("Surface-Extrude1""BODYFEATURE", 0, 0, 0, false, 0, null, 0);
 
            slotDepth = 0.01;
            slotWidth = 0.04;
            slotLength = 0.09;
            slotThruAll = false;
            halfWidth = slotWidth / 2;
            halfLength = slotLength / 2;
            ptArr[0] = 0.0;
            ptArr[1] = 0.0;
            ptArr[2] = 0.0;
            dirArr[0] = 0.0;
            dirArr[1] = 0.0;
            dirArr[2] = 1.0;
            startArr[0] = 1.0;
            startArr[1] = 0.0;
            startArr[2] = 0.0;
            planeSurf = (Surface)swModeler.CreatePlanarSurface2((ptArr), (dirArr), (startArr));
 
            ptArr[0] = -halfLength;
            ptArr[1] = halfWidth;
            ptArr[2] = 0.0;
            dirArr[0] = 1.0;
            dirArr[1] = 0.0;
            dirArr[2] = 0.0;
            trimCurves[0] = (Curve)swModeler.CreateLine((ptArr), (dirArr));
            trimCurves[0] = (Curve)trimCurves[0].CreateTrimmedCurve2(-halfLength, halfWidth, 0.0, halfLength, halfWidth, 0.0);
 
            ptArr[0] = halfLength;
            ptArr[1] = 0.0;
            ptArr[2] = 0.0;
            startArr[0] = halfLength;
            startArr[1] = halfWidth;
            startArr[2] = 0.0;
            endArr[0] = halfLength;
            endArr[1] = -halfWidth;
            endArr[2] = 0.0;
            dirArr[0] = 0.0;
            dirArr[1] = 0.0;
            dirArr[2] = -1.0;
            trimCurves[1] = (Curve)swModeler.CreateArc((ptArr), (dirArr), halfWidth, (startArr), (endArr));
            trimCurves[1] = (Curve)trimCurves[1].CreateTrimmedCurve2(halfLength, halfWidth, 0.0, halfLength, -halfWidth, 0.0);
 
            ptArr[0] = halfLength;
            ptArr[1] = -halfWidth;
            ptArr[2] = 0.0;
            dirArr[0] = -1.0;
            dirArr[1] = 0.0;
            dirArr[2] = 0.0;
            trimCurves[2] = (Curve)swModeler.CreateLine((ptArr), (dirArr));
            trimCurves[2] = (Curve)trimCurves[2].CreateTrimmedCurve2(halfLength, -halfWidth, 0.0, -halfLength, -halfWidth, 0.0);
 
            ptArr[0] = -halfLength;
            ptArr[1] = 0.0;
            ptArr[2] = 0.0;
            startArr[0] = -halfLength;
            startArr[1] = -halfWidth;
            startArr[2] = 0.0;
            endArr[0] = -halfLength;
            endArr[1] = halfWidth;
            endArr[2] = 0.0;
            dirArr[0] = 0.0;
            dirArr[1] = 0.0;
            dirArr[2] = -1.0;
            trimCurves[3] = (Curve)swModeler.CreateArc((ptArr), (dirArr), halfWidth, (startArr), (endArr));
            trimCurves[3] = (Curve)trimCurves[3].CreateTrimmedCurve2(-halfLength, -halfWidth, 0.0, -halfLength, halfWidth, 0.0);
            profileBody = (Body2)planeSurf.CreateTrimmedSheet((trimCurves));
 
            dirArr[0] = 0.0;
            dirArr[1] = 0.0;
            dirArr[2] = -1.0;
            dirVector = (MathVector)swMath.CreateVector((dirArr));
            extrudedBody = (Body2)swModeler.CreateExtrudedBody(profileBody, dirVector, slotDepth);
            extrudedBody.Display3(swModel, Information.RGB(1, 0, 0), (int)swTempBodySelectOptions_e.swTempBodySelectOptionNone); 
 
        }
 
        /// <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 Temporary Extruded Body 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) 2018 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.