Hide Table of Contents

Create and Access Curve-driven Pattern Feature Example (C#)

This example shows how to create a curve-driven pattern feature and access its data.

//--------------------------------------------------------------
// Preconditions:
// 1. Verify that the specified part document to open exists.
// 2. Open the Immediate window.
//
// Postconditions:
// 1. Opens the specified part document.
// 2. Creates a cut extrude feature.
// 3. Creates a curve-driven pattern feature using the
//    the cut extrude feature.
// 4. Gets curve-driven pattern feature data.
// 5. Examine the FeatureManager design tree, graphics area,
//    and Immediate window.
//
// NOTE: Because the part is used elsewhere, do not save changes.
//--------------------------------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
using System.Diagnostics;
 
namespace CurveDrivenPatternFeatureCSharp.csproj
{
    public partial class SolidWorksMacro
    {
 
        public void Main()
        {
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            SketchManager swSketchMgr = default(SketchManager);
            SketchSegment swSketchSegment = default(SketchSegment);
            FeatureManager swFeatureMgr = default(FeatureManager);
            Feature swFeature = default(Feature);
            SelectionMgr swSelectionMgr = default(SelectionMgr);
            CurveDrivenPatternFeatureData swCurveDrivenPatternFeatureData = default(CurveDrivenPatternFeatureData);
            Entity swEntity = default(Entity);
            object patternDirection = null;
            string fileName = null;
            bool status = false;
            int errors = 0;
            int warnings = 0;
 
            fileName = "C:\\Program Files\\SolidWorks Corp\\SolidWorks\\samples\\tutorial\\api\\bagel.sldprt";
            swModel = (ModelDoc2)swApp.OpenDoc6(fileName, (int)swDocumentTypes_e.swDocPART, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, ""ref errors, ref warnings);
 
            //Sketch a circle and create a cut extrude
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            status = swModelDocExt.SelectByID2("""FACE", 0.0118560192339032, 0, 0.0566664535234693, false, 0, null, 0);
            swSketchMgr = (SketchManager)swModel.SketchManager;
            swSketchMgr.InsertSketch(true);
            swSketchSegment = (SketchSegment)swSketchMgr.CreateCircle(-0.059172, -0.048012, 0.0, -0.044189, -0.040533, 0.0);
            swSketchMgr.InsertSketch(true);
            swModel.ClearSelection2(true);
            status = swModelDocExt.SelectByID2("Sketch6""SKETCH", 0, 0, 0, false, 0, null, 0);
            swFeatureMgr = (FeatureManager)swModel.FeatureManager;
            swFeature = (Feature)swFeatureMgr.FeatureCut3(truefalsefalse, 1, 0, 0.00254, 0.00254, falsefalsefalse,
            false, 0.0174532925199433, 0.0174532925199433, falsefalsefalsefalsefalsetruetrue,
            truetruefalse, 0, 0, false);
            swSelectionMgr = (SelectionMgr)swModel.SelectionManager;
            swSelectionMgr.EnableContourSelection = false;
            swModel.ActivateSelectedFeature();
            status = swModelDocExt.SelectByID2("""EDGE", 0.0115207253109588, -8.89643058599177E-06, 0.0754182969300832, true, 0, null, 0);
            swModel.ClearSelection2(true);
 
            //Create curve-driven pattern feature
            status = swModelDocExt.SelectByID2("Cut-Extrude2""BODYFEATURE", 0, 0, 0, false, 4, null, 0);
            status = swModelDocExt.SelectByID2("""EDGE", 0.0115207253109588, -8.89643058599177E-06, 0.0754182969300832, true, 1, null, 0);
            swModel.FeatureCurvePattern(3, 0.0254, 1, 0.00254, falsefalsefalsefalsetruefalse,
            falsefalse);
 
            //Access the curve-driven pattern feature
            status = swModelDocExt.SelectByID2("CrvPattern1""BODYFEATURE", 0, 0, 0, false, 0, null, 0);
            swFeature = (Feature)swSelectionMgr.GetSelectedObject6(1, -1);
            swCurveDrivenPatternFeatureData = (CurveDrivenPatternFeatureData)swFeature.GetDefinition();
            status = swCurveDrivenPatternFeatureData.AccessSelections(swModel, null);
            Debug.Print("Number of pattern instances in Direction 1: " + swCurveDrivenPatternFeatureData.D1InstanceCount);
            Debug.Print("Alignment method of Direction 1: " + swCurveDrivenPatternFeatureData.D1AlignmentMethod);
            Debug.Print("Curve method of Direction 1: " + swCurveDrivenPatternFeatureData.D1CurveMethod);
            patternDirection = swCurveDrivenPatternFeatureData.D1Direction;
            swEntity = (Entity)patternDirection;
            Debug.Print("Pattern direction object type of Direction 1: " + swEntity.GetType());
            Debug.Print("Pattern instances spaced equally in Direction 1? " + swCurveDrivenPatternFeatureData.D1IsEqualSpaced);
            Debug.Print("Pattern direction reversed in Direction 1? " + swCurveDrivenPatternFeatureData.D1ReverseDirection);
            Debug.Print("Number of seed bodies in pattern: " + swCurveDrivenPatternFeatureData.GetPatternBodyCount());
            Debug.Print("Number of seed features in pattern: " + swCurveDrivenPatternFeatureData.GetPatternFeatureCount());
            swCurveDrivenPatternFeatureData.ReleaseSelectionAccess();
 
        }
 
        /// <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 and Access Curve-driven Pattern Feature 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) 2016 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.