Hide Table of Contents

Create Loft Body Example (C#)

This example shows how to create a temporary loft body using IModeler::CreateLoftBody2.

//-----------------------------------------------------
// Preconditions:
// 1. Verify that the specified part document template
//    exists.
// 2. Open the Immediate window.
//
// Postconditions:
// 1. Opens a new part document.
// 2. Creates and selects sketches of two profiles and
//    a guide curve.
// 3. Creates a temporary loft body.
// 4. Examine the Immediate window and graphics area.
//-----------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
using System.Diagnostics;
 
namespace CreateLoftCSharp.csproj
{
    public partial class SolidWorksMacro
    {
 
 
        public void Main()
        {
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            SketchManager swSketchMgr = default(SketchManager);
            SketchSegment sketchSegment = default(SketchSegment);
            SelectionMgr swSelMgr = default(SelectionMgr);
            SketchPoint sketchPoint = default(SketchPoint);
            FeatureManager swFeatureMgr = default(FeatureManager);
            RefPlane refPlane = default(RefPlane);
            Feature swFeat = default(Feature);
            bool status = false;
            object profiles = null;
            object guides = null;
            Feature[] profile = new Feature[2];
            Feature[] guideCurve = new Feature[1];
            Modeler swModeler = default(Modeler);
            Body2 swBody = default(Body2);
            int count = 0;
            object[] featArr = null;
            int i = 0;
 
            //Open new part document
            swModel = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SolidWorks\\SolidWorks 2014\\templates\\Part.prtdot", 0, 0, 0);
            swModelDocExt = (ModelDocExtension)swModel.Extension;
 
            //Create closed profile
            status = swModelDocExt.SelectByID2("Front Plane""PLANE", 0, 0, 0, false, 0, null, 0);
            swSketchMgr = (SketchManager)swModel.SketchManager;
            sketchSegment = (SketchSegment)swSketchMgr.CreateCircle(0.0, 0.0, 0.0, 0.021796, -0.030937, 0.0);
            sketchPoint = (SketchPoint)swSketchMgr.CreatePoint(0.023454, 0.029699, 0.0);
            swModel.ClearSelection2(true);
            swSketchMgr.InsertSketch(true);
 
            //Create another closed profile
            status = swModelDocExt.SelectByID2("Front Plane""PLANE", 0, 0, 0, true, 0, null, 0);
            swFeatureMgr = (FeatureManager)swModel.FeatureManager;
            refPlane = (RefPlane)swFeatureMgr.InsertRefPlane(8, 0.254, 0, 0, 0, 0);
            status = swModelDocExt.SelectByID2("Plane1""PLANE", 0, 0, 0, false, 0, null, 0);
            sketchSegment = (SketchSegment)swSketchMgr.CreateCircle(-0.035118, -0.014102, 0.0, -0.025452, -0.02953, 0.0);
            sketchPoint = (SketchPoint)swSketchMgr.CreatePoint(-0.018033, -0.020392, 0.0);
            swModel.ClearSelection2(true);
            swSketchMgr.InsertSketch(true);
 
            //Create guide curve
            status = swModelDocExt.SelectByID2("Point4@Sketch1""EXTSKETCHPOINT", 0.0234541440502721, 0.0296993303358475, 0, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("Point5@Sketch2""EXTSKETCHPOINT", -0.0180330744027628, -0.0203923494843098, 0, true, 0, null, 0);
            swModel.ClearSelection2(true);
            status = swModelDocExt.SelectByID2("Point4@Sketch1""EXTSKETCHPOINT", 0.0234541440502721, 0.0296993303358475, 0, false, 1, null, 0);
            status = swModelDocExt.SelectByID2("Point5@Sketch2""EXTSKETCHPOINT", -0.0180330744027628, -0.0203923494843098, 0, true, 1, null, 0);
            swModel.Insert3DSplineCurve(false);
            swModel.ClearSelection2(true);
 
            //Select guide curve and profiles for loft feature
            status = swModelDocExt.SelectByID2("Curve1""REFERENCECURVES", 0, 0, 0, false, 2, null, 0);
            swSelMgr = (SelectionMgr)swModel.SelectionManager;
            swFeat = (Feature)swSelMgr.GetSelectedObject6(1, -1);
            Debug.Print("Guide curve name: " + swFeat.Name);
            guideCurve[0] = (Feature)swFeat;
            guides = guideCurve;
            swModel.ClearSelection2(true);
            status = swModelDocExt.SelectByID2("Sketch1""SKETCH", 0.00984860021145358, 0.0365397341178567, 0, true, 1, null, 0);
            swFeat = (Feature)swSelMgr.GetSelectedObject6(1, -1);
            Debug.Print("Profile name: " + swFeat.Name);
            profile[0] = (Feature)swFeat;
            swModel.ClearSelection2(true);
            status = swModelDocExt.SelectByID2("Sketch2""SKETCH", -0.0401969362026636, 0.00338231877308527, 0, true, 1, null, 0);
            swFeat = (Feature)swSelMgr.GetSelectedObject6(1, -1);
            Debug.Print("Profile name: " + swFeat.Name);
            profile[1] = (Feature)swFeat;
            profiles = profile;
            swModel.ClearSelection2(true);
 
            //Create temporary loft body
            swModeler = (Modeler)swApp.GetModeler();
            swBody = (Body2)swModeler.CreateLoftBody2(swModel, profiles, guides, nullfalse, 0, 0, 0, truefalse,
            truefalsetrue, 1, 1, 1, truetrue, 1, 1,
            false);
 
            // Test whether the loft body is a temporary body
            status = swBody.IsTemporaryBody();
            Debug.Print("Is the loft body a temporary body?  " + status);
            if (status)
            {
                // Display the temporary loft body
                swBody.Display3(swModel, 256, (int)swTempBodySelectOptions_e.swTempBodySelectOptionNone);
                Debug.Print("Temporary loft body displayed; examine the graphics area.");
            }
            else
            {
                Debug.Print("Temporary loft body was not created.");
            }
 
            Debug.Print("");
 
            //Verify that the temporary loft body is not a loft feature
            //by examining the list of features printed to the
            //Immediate window
            count = swFeatureMgr.GetFeatureCount(false);
            featArr = (object[])swFeatureMgr.GetFeatures(false);
            for (i = 0; i < count - 1; i++)
            {
                swFeat = (Feature)featArr[i];
                Debug.Print(swFeat.Name);
            }
 
            swModel.ViewZoomtofit2();
 
        }
 
        /// <summary>
        ///  The SldWorks swApp variable is pre-assigned for you.
        /// </summary>
        public SldWorks swApp;
    }
}


Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Create Loft Body Example (C#)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:




x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2015 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.