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Create Library Feature Data Object and Library Feature With References Example (C#)

This example shows how to create a library feature with references in order to position the library feature on a model.

//------------------------------------------------------
// Preconditions:
// 1. Verify that the specified part template and library feature
//    exist.
// 2. Open the Immediate window.
//
// Postconditions:
// 1. Creates a new part containing a boss extrude.
// 2. Creates a library feature data object.
//    a. Initializes the newly created library feature using
//       the specified library feature.
//    b. Gets the type of references required for the library
//       feature.
//    c. Sets the name of the active library feature configuration.
//    d. Selects the face where to create the library feature.
//    e. Creates the library feature.
//    f. Accesses the library feature and selects the edges where to
//       position the it.
//    g. Sets the references for positioning the library feature.
//    h. Updates the definition of the library feature.
//    i. Unsuppresses the library feature.
// 3. Examine the Immediate window, FeatureManager design tree, and
//    graphics area.
//-------------------------------------------------------
 
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System;
using System.Diagnostics;
using System.Runtime.InteropServices;
 
namespace Macro1CSharp.csproj
{
    partial class SolidWorksMacro
    {
        public void Main()
        {
            Feature swFeature = default(Feature);
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            SketchManager swSketchManager = default(SketchManager);
            SelectionMgr swSelectionManager = default(SelectionMgr);
            FeatureManager swFeatureManager = default(FeatureManager);
            LibraryFeatureData swLibFeat = default(LibraryFeatureData);
            bool status = false;
            object[] sketchLines = null;
            object Refs = null;
            object RefTypes = null;
            int RefCount = 0;
            int k = 0;
            int i = 0;
            DispatchWrapper[] LibRefs = null;
 
            // Create part
            swModel = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SolidWorks\\SOLIDWORKS 2016\\templates\\Part.prtdot", 0, 0, 0);
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            status = swModelDocExt.SelectByID2("Top Plane""PLANE", 0, 0, 0, false, 0, null, 0);
            swModel.ClearSelection2(true);
            status = swModelDocExt.SetUserPreferenceToggle((int)swUserPreferenceToggle_e.swSketchAddConstToRectEntity, (int)swUserPreferenceOption_e.swDetailingNoOptionSpecified, false);
            status = swModelDocExt.SetUserPreferenceToggle((int)swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, (int)swUserPreferenceOption_e.swDetailingNoOptionSpecified, true);
            swSketchManager = (SketchManager)swModel.SketchManager;
            sketchLines = (object[])swSketchManager.CreateCornerRectangle(0, 0, 0, 1, 0.5, 0);
            swModel.ShowNamedView2("*Trimetric", 8);
            swModel.ClearSelection2(true);
            status = swModelDocExt.SelectByID2("Line2""SKETCHSEGMENT", 0, 0, 0, false, 0, null, 0);
            status = swModelDocExt.SelectByID2("Line1""SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("Line4""SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("Line3""SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            swFeatureManager = (FeatureManager)swModel.FeatureManager;
            swFeature = (Feature)swFeatureManager.FeatureExtrusion2(truefalsefalse, 0, 0, 0.01, 0.01, falsefalsefalse,
            false, 0.0174532925199433, 0.0174532925199433, falsefalsefalsefalsetruetruetrue,
            0, 0, false);
            swSelectionManager = (SelectionMgr)swModel.SelectionManager;
            swSelectionManager.EnableContourSelection = false;
 
            // Create library feature 
            swLibFeat = (LibraryFeatureData)swFeatureManager.CreateDefinition((int)swFeatureNameID_e.swFmLibraryFeature);
 
            // Initialize newly created library feature using the specified library part 
            status = swLibFeat.Initialize("C:\\ProgramData\\SOLIDWORKS\\SOLIDWORKS 2016\\design library\\features\\metric\\slots\\straight slot.sldlfp");
 
            // Get the type of references required for the library feature 
            RefCount = swLibFeat.GetReferencesCount();
            Refs = (object[])swLibFeat.GetReferences2((int)swLibFeatureData_e.swLibFeatureData_FeatureRespect, out RefTypes);
 
            if ((RefTypes != null))
            {
                Debug.Print("Types of references required (edge = 1): ");
                int[] RefType = (int[])RefTypes;
                for (k = RefType.GetLowerBound(0); k <= RefType.GetUpperBound(0); k++)
                {
                    Debug.Print("    " + RefType[k].ToString());
                }
            }
 
 
            // Set the name of the active library feature configuration 
            swLibFeat.ConfigurationName = "Default";
 
            // Select the face where to create the library feature 
            status = swModelDocExt.SelectByID2("""FACE", 0.522458766456054, 0.288038964184011, 0.00999999999987722, false, 0, null, 0);
 
            // Create the library feature 
            swFeature = (Feature)swFeatureManager.CreateFeature(swLibFeat);
 
            // Access the library feature to position it on the part 
            swLibFeat = null;
            swLibFeat = (LibraryFeatureData)swFeature.GetDefinition();
            status = swLibFeat.AccessSelections(swModel, null);
 
            // Select the edges where to position the library feature
            status = swModelDocExt.SelectByID2("""EDGE", 0.960865149149924, 0.497807163546383, 0.0131011390528215, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("""EDGE", 0.99866860703213, 0.481385806014544, 0.0113313929676906, true, 0, null, 0);
 
            int selCount = 0;
            selCount = swSelectionManager.GetSelectedObjectCount2(-1);
 
            object[] selectedObjects = new object[selCount];
 
            for (i = 0; i < selCount; i++)
            {
                object selectedObject = null;
                selectedObject = (object)swSelectionManager.GetSelectedObject6(i + 1, -1);
                selectedObjects[i] = selectedObject;
            }
 
            // Convert the .NET array to IDispatch
            LibRefs = (DispatchWrapper[])ObjectArrayToDispatchWrapperArray((selectedObjects));
 
            // Set the references for positioning the library feature on the part 
            swLibFeat.SetReferences(LibRefs);
 
            // Update the definition of the library feature 
            status = swFeature.ModifyDefinition(swLibFeat, swModel, null);
 
            // Unsuppress the library feature
            status = swModelDocExt.SelectByID2("straight slot<1>""BODYFEATURE", 0, 0, 0, false, 0, null, 0);
            swModel.EditUnsuppress2();
 
            swModel.ClearSelection2(true);
        }
 
        public DispatchWrapper[] ObjectArrayToDispatchWrapperArray(object[] Objects)
        {
            int ArraySize = 0;
            ArraySize = Objects.GetUpperBound(0);
            DispatchWrapper[] d = new DispatchWrapper[ArraySize + 1];
            int ArrayIndex = 0;
            for (ArrayIndex = 0; ArrayIndex <= ArraySize; ArrayIndex++)
            {
                d[ArrayIndex] = new DispatchWrapper(Objects[ArrayIndex]);
            }
            return d;
        }
 
 
        /// <summary> 
        /// The SldWorks swApp variable is pre-assigned for you. 
        /// </summary> 
        public SldWorks swApp;
        public DispatchWrapper[] LibRefs;
 
 
    }
}


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