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Add Attribute to Feature and Include in Library Feature Example (C#)

This example shows how to add an attribute to a feature and include that attribute with the feature if the feature is saved as a library feature. This example also includes instructions on how to verify that the attribute is included on each instance of the library feature.

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

// Preconditions:

//   1. Open a new part document.

//   2. Sketch a rectangle and extrude it.

//   3. Sketch a straight slot that fits on a face of

//       of the just-created extrude and cut-extrude the slot.

//       The cut-extrude should be named Extrude2.

//

// Postconditions: The Extrude2 feature is added to the part document with

//                an attribute of TestAttribute, which is visible in the

//                FeatureManager design tree.

//

// To verify that the attribute is included in a library feature:

//   1. Drag the Extrude2 feature to the Design Library and

//      save the library feature.

//   2. Close, and optionally save, the part document.

//   3. Open a model document and drag-and-drop the just-created library

//      feature on the model.

//   4. Expand the just-dropped library feature in the FeatureManager design

//      tree.

//

//      Extrude2 and TestAttribute should appear beneath the

//      just-dropped library feature in the FeatureManager design tree.

//

//   5. Close, and optionally save, the model document.

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

using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

using System.Diagnostics;

using System;

namespace AddAttributesToFeature_CSharp.csproj

{

    partial class SolidWorksMacro

    {

        public void Main()

        {

            ModelDoc2 swModel = default(ModelDoc2);

            ModelDocExtension swModelDocExt = default(ModelDocExtension);

            SelectionMgr swSelectionMgr = default(SelectionMgr);

            Feature swFeature = default(Feature);

            SolidWorks.Interop.sldworks.Attribute swAttribute = default(SolidWorks.Interop.sldworks.Attribute);

            AttributeDef swAttributeDef = default(AttributeDef);

            Face2 swFace = default(Face2);

            Object[] Faces = null;

            bool @bool = false;

            swModel = (ModelDoc2)swApp.ActiveDoc;

            swModelDocExt = swModel.Extension;

            swSelectionMgr = (SelectionMgr)swModel.SelectionManager;

            // Create attribute

            swAttributeDef = (AttributeDef)swApp.DefineAttribute("TestPropagationOfAttribute");

            @bool = swAttributeDef.AddParameter("TestAttribute", (int)swParamType_e.swParamTypeDouble, 2.0, 0);

            @bool = swAttributeDef.Register();

            // Select the feature to which to add the attribute

            @bool = swModelDocExt.SelectByID2("Extrude2", "BODYFEATURE", 0, 0, 0, false, 0, null, 0);

            swFeature = (Feature)swSelectionMgr.GetSelectedObject6(1, -1);

            Debug.Print("Name of feature to which to add attribute: " + swFeature.Name);

            // Add the attribute to one of the feature's faces

            Faces = (Object[])swFeature.GetFaces();

            swFace = (Face2)Faces[0];

            swAttribute = swAttributeDef.CreateInstance5(swModel, swFace, "TestAttribute", 0, (int)swInConfigurationOpts_e.swAllConfiguration);

            swAttribute.IncludeInLibraryFeature = true;

            Debug.Print("Include attribute in library feature? " + swAttribute.IncludeInLibraryFeature);

            swModel.ForceRebuild3(false);

        }

        public SldWorks swApp;

    }

}       



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