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Set Body for View Example (C#)

This example shows how to show just one body of a multibody part in a drawing view.

// Preconditions:
// 1. Open public_documents\tutorial\multibody\multi_inter.sldprt.
// 2. Save the part document as a drawing document:
//    a. Click File > Make Drawing from Part.
//    b. Click OK on the Sheet Format/Size dialog.
//    c. Drag the *Isometric view from the View Palette onto
//       the drawing sheet.
// 3. Select the drawing view.
// 4. Open the Immediate window.
// Postconditions:
// 1. Shows one body of the multibody part
//    in the drawing view.
// 2. Examine the drawing and the Immediate window.
// NOTE: Because the part document is used elsewhere, do not save
// changes.

using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

using System;

using System.Diagnostics;

using System.Runtime.InteropServices;

using System.Windows.Forms;

namespace BodiesViewCSharp.csproj


    partial class SolidWorksMacro


        public void Main()


            ModelDoc2 swModel = default(ModelDoc2);

            SelectionMgr swSelMgr = default(SelectionMgr);

            SolidWorks.Interop.sldworks.View swView = default(SolidWorks.Interop.sldworks.View);

            int nbrBodies = 0;

            object[] arrBody = null;

            Body2 swBody = default(Body2);

            Face2 swFace = default(Face2);

            Entity swEnt = default(Entity);

            SelectData swSelData = default(SelectData);

            PartDoc swPart = default(PartDoc);

            bool status = false;

            DispatchWrapper[] arrBodiesIn = new DispatchWrapper[1];

            object[] Bodies = new object[1];

            int i = 0;

            int objType = 0;


            swModel = (ModelDoc2)swApp.ActiveDoc;

            swSelMgr = (SelectionMgr)swModel.SelectionManager;

            swView = (SolidWorks.Interop.sldworks.View)swSelMgr.GetSelectedObject6(1, -1);

            if ((swView == null))


                MessageBox.Show("View not selected.");



            nbrBodies = swView.GetBodiesCount();

            Debug.Print("Number of bodies: " + nbrBodies);

            if ((nbrBodies < 1))


                MessageBox.Show("No bodies in selected view.");



            arrBody = (object[])swView.Bodies;

            for (i = 0; i < arrBody.Length; i++)


                swBody = (Body2)arrBody[i];

                swSelData = (SelectData)swSelMgr.CreateSelectData();

                swSelData.View = swView;

                status = swBody.Select2(false, swSelData);

                // Object type 76 is a solid body

                objType = swSelMgr.GetSelectedObjectType3(1, -1);

                if ((objType == 76))


                    Debug.Print(" Object type: solid body");


                if ((!((int)swSelectType_e.swSelSOLIDBODIES == swSelMgr.GetSelectedObjectType3(1, -1))))


                    MessageBox.Show("Solid body not found.");


                swFace = (Face2)swBody.GetFirstFace();

                while ((swFace != null))


                    swEnt = (Entity)swFace;

                    // Select using IEntity

                    status = swEnt.Select4(true, swSelData);


                    swFace = (Face2)swFace.GetNextFace();


                Debug.Print(" Name of body: " + swBody.GetSelectionId());





            // Get the bodies from referenced model

            swModel = (ModelDoc2)swView.ReferencedDocument;

            swPart = (PartDoc)swModel;

            arrBody = (object[])swPart.GetBodies2((int)swBodyType_e.swSolidBody, true);

            if ((nbrBodies == 1))


                swView.Bodies = (arrBody);




                // Set the body to include in the drawing view

                Bodies[0] = arrBody[0];

                arrBodiesIn[0] = new DispatchWrapper(Bodies[0]);

                swView.Bodies = (arrBodiesIn);






        /// <summary>

        /// The SldWorks swApp variable is pre-assigned for you.

        /// </summary>

        public SldWorks swApp;




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