Select Multiple Splines for Loft Guide Curves Example (C#)

This example shows how to select multiple splines for the guide curves for a loft feature.

//---------------------------------------------------------------
// Preconditions: Verify that the specified part template exists.
//
// Postconditions:
// 1. Creates a new part.
// 2. Creates a profile sketch.
// 3. Creates a reference plane and another profile sketch on that
//    reference plane.
// 4. Creates two splines for the guide curves.
// 5. Selects the profile sketches.
// 6. Selects the splines and groups them as an object.
// 7. Creates a loft feature.
// 8. Examine the FeatureManager design tree and graphics area.
//---------------------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
 
namespace Macro1CSharp.csproj
{
    public partial class SolidWorksMacro
    {
        public void Main()
        {
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            SketchSegment swSketchSegment = default(SketchSegment);
            SketchManager swSketchManager = default(SketchManager);
            RefPlane swRefPlane = default(RefPlane);
            FeatureManager swFeatureManager = default(FeatureManager);
            bool status = false;
 
            //Create a new part
            swModel = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SolidWorks\\SOLIDWORKS 2017\\templates\\Part.prtdot", 0, 0, 0);
 
            //Create a profile sketch
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, false, 0, null, 0);
            swModel.ClearSelection2(true);
            swSketchManager = (SketchManager)swModel.SketchManager;
            swSketchSegment = (SketchSegment)swSketchManager.CreateEllipse(0, 0, 0, 0.0706113079019074, 0, 0, 0, 0.0374944141689373, 0);
            swModel.ClearSelection2(true);
            swSketchManager.InsertSketch(true);
 
            //Create a reference plane and another profile sketch
            //on that reference plane
            status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, true, 0, null, 0);
            swFeatureManager = (FeatureManager)swModel.FeatureManager;
            swRefPlane = (RefPlane)swFeatureManager.InsertRefPlane(8, 0.07, 0, 0, 0, 0);
            swModel.ClearSelection2(true);
            status = swModelDocExt.SelectByID2("Plane1", "PLANE", 0, 0, 0, false, 0, null, 0);
            swSketchSegment = (SketchSegment)swSketchManager.CreateEllipse(0, 0, 0, 0.0527205722070845, 0, 0, 0, 0.0154164850136235, 0);
            swModel.ClearSelection2(true);
            swSketchManager.InsertSketch(true);
 
            //Create a spline
            status = swModelDocExt.SelectByID2("Right Plane", "PLANE", 0, 0, 0, false, 0, null, 0);
            object pointArray = null;
            double[] points = new double[15];
            points[0] = -0.07;
            points[1] = 0.0154164850136235;
            points[2] = 0;
            points[3] = -0.0531092941649547;
            points[4] = 0.0280386111480766;
            points[5] = 0;
            points[6] = -0.0296934467839947;
            points[7] = 0.0229795168190776;
            points[8] = 0;
            points[9] = -0.0112921067380967;
            points[10] = 0.026354325474415;
            points[11] = 0;
            points[12] = 0;
            points[13] = 0.0374944141689373;
            points[14] = 0;
            pointArray = points;
            swSketchSegment = (SketchSegment)swSketchManager.CreateSpline((pointArray));
            swSketchManager.InsertSketch(true);
            swModel.ClearSelection2(true);
 
            //Create another spline
            status = swModelDocExt.SelectByID2("Right Plane", "PLANE", 0, 0, 0, false, 0, null, 0);
            points = new double[9];
            points[0] = -0.07;
            points[1] = -0.0154164850136235;
            points[2] = 0;
            points[3] = -0.0307689275649068;
            points[4] = -0.0233694015292372;
            points[5] = 0;
            points[6] = 0;
            points[7] = -0.0374944141689373;
            points[8] = 0;
            pointArray = points;
            swSketchSegment = swSketchManager.CreateSpline((pointArray));
            swSketchManager.InsertSketch(true);
            swModel.ClearSelection2(true);
 
            //Select the profile sketches
            status = swModelDocExt.SelectByID2("Sketch1", "SKETCH", -0.0585496337278505, 0.0209585732143712, 1, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("Sketch2", "SKETCH", -0.0379093739088495, 0.0107136192740755, 1, true, 0, null, 0);
 
            //Select the splines for the guide curves
            status = swModelDocExt.SelectByID2("Spline1@Sketch3", "EXTSKETCHSEGMENT", -0.00620659823337474, 0.0304187689522769, 2, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("Spline1@Sketch4", "EXTSKETCHSEGMENT", -0.0402947949143199, -0.0206106896601265, 2, true, 0, null, 0);
            //Group the selected splines as an object
            status = swModelDocExt.SelectByID2("Unknown", "SELOBJGROUP", 0, 0, 0, true, 2, null, 0);
 
            //Create a loft
            swFeatureManager.InsertProtrusionBlend2(false, true, false, 1, 0, 0, 1, 1, true, true,
            false, 0, 0, 0, true, true, true, 0); 
 
 
        }
 
        /// <summary>
        ///  The SldWorks swApp variable is pre-assigned for you.
        /// </summary>
        public SldWorks swApp;
    }
}