Get Bodies in Components Example (C#)

This example shows how to get the number of normal and user bodies in the components in an assembly.

//-------------------------------------

// Preconditions:

// 1. Specified assembly document exists.

// 2. Run the macro.

//

// Postconditions: Each component's name, number of

// solid bodies, body names, and body types are

// printed to the Immediate window.

//

// To understand the results of the macro:

// 1. Right-click filterholder in the FeatureManager

//    design tree and click the Open Part button in

//    the context toolbar. Notice that there

//    are no screw holes in the part.

// 2. Close the part and examine the filterholder

//    component, which is the orange, flat, circular

//    component located on the front of the assembly,

//    in the graphics area. There are screw

//    holes in the component.

// 3. Locate filterholder's information in the

//    Immediate window. Because the component was

//    modified in the assembly, its body is identified

//    as a user body.

//

// NOTE: Because this assembly 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;

using System.Diagnostics;

using System.Collections;

namespace GetBodies3Component2CSharp.csproj

{

partial class SolidWorksMacro

{

    public void Main()

    {

        ModelDoc2 swModel = default(ModelDoc2);

        AssemblyDoc swAssembly = default(AssemblyDoc);

        object[] vComponents = null;

        Component2 oneComponent = default(Component2);

        Body2 swBody = default(Body2);

        object[] vBodies = null;

        object vBodyInfo;

        int[] BodiesInfo = null;

        int BodyType = 0;

        int errors = 0;

        int warnings = 0;

        int i = 0;

        int j = 0;

 

        // Open this assembly or substitute the path and name of your assembly here

        swModel = (ModelDoc2)swApp.OpenDoc6("C:\\Program Files\\SolidWorks Corp\\SolidWorks\\samples\\tutorial\\toolbox\\lens_mount.sldasm", (int)swDocumentTypes_e.swDocASSEMBLY, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, "", ref errors, ref warnings);

        swAssembly = (AssemblyDoc)swModel;

 

        // Get the components in the assembly

        vComponents = (object[])swAssembly.GetComponents(true);

        for (i = 0; i <= vComponents.Length-1; i++)

        {

            oneComponent = (Component2)vComponents[i];

            Debug.Print(" ");

            Debug.Print("Component name: " + oneComponent.Name2);

 

            // Get the solid bodies in the component

            vBodies = (object[])oneComponent.GetBodies3((int)swBodyType_e.swSolidBody, out (object)vBodyInfo);

            BodiesInfo = (int[])vBodyInfo;

            Debug.Print(" Number of solid bodies: " + (vBodies.Length + 1));

            for (j = 0; j <= vBodies.Length-1; j++)

            {

                Debug.Print(" Body number: " + (j + 1));

                swBody = (Body2)vBodies[j];

                Debug.Print(" Body name: " + swBody.Name);

 

                // Print the type of body

                BodyType = (int)BodiesInfo[j];

                switch (BodyType)

                {

                    case 0:

                        Debug.Print(" Body type: user");

                        break;

                    case 1:

                        Debug.Print(" Body type: normal");

                        break;

                }

            }

        }

    }

 

    /// <summary>

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

    /// </summary>

    public SldWorks swApp;

 

}

}