Hide Table of Contents

Create and Access Curve-driven Pattern Feature Example (VB.NET)

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

' Preconditions:
' 1. Verify that the specified part 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.
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
Partial Class SolidWorksMacro
    Public Sub main()
        Dim swModel As ModelDoc2
        Dim swModelDocExt As ModelDocExtension
        Dim swSketchMgr As SketchManager
        Dim swSketchSegment As SketchSegment
        Dim swFeatureMgr As FeatureManager
        Dim swFeature As Feature
        Dim swSelectionMgr As SelectionMgr
        Dim swCurveDrivenPatternFeatureData As CurveDrivenPatternFeatureData
        Dim swEntity As Entity
        Dim patternDirection As Object
        Dim fileName As String
        Dim status As Boolean
        Dim errors As Integer
        Dim warnings As Integer
        fileName = "C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\api\bagel.sldprt"
        swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
        'Sketch a circle and create a cut extrude
        swModelDocExt = swModel.Extension
        status = swModelDocExt.SelectByID2("""FACE", 0.0118560192339032, 0, 0.0566664535234693, False, 0, Nothing, 0)
        swSketchMgr = swModel.SketchManager
        swSketchSegment = swSketchMgr.CreateCircle(-0.059172, -0.048012, 0.0#, -0.044189, -0.040533, 0.0#)
        status = swModelDocExt.SelectByID2("Sketch6""SKETCH", 0, 0, 0, False, 0, Nothing, 0)
        swFeatureMgr = swModel.FeatureManager
        swFeature = swFeatureMgr.FeatureCut3(TrueFalseFalse, 1, 0, 0.00254, 0.00254, FalseFalseFalseFalse, 0.0174532925199433, 0.0174532925199433, FalseFalseFalseFalseFalseTrueTrueTrueTrueFalse, 0, 0, False)
        swSelectionMgr = swModel.SelectionManager
        swSelectionMgr.EnableContourSelection = False
        status = swModelDocExt.SelectByID2("""EDGE", 0.0115207253109588, -0.00000889643058599177, 0.0754182969300832, True, 0, Nothing, 0)
        'Create curve-driven pattern feature
        status = swModelDocExt.SelectByID2("Cut-Extrude2""BODYFEATURE", 0, 0, 0, False, 4, Nothing, 0)
        status = swModelDocExt.SelectByID2("""EDGE", 0.0115207253109588, -0.00000889643058599177, 0.0754182969300832, True, 1, Nothing, 0)
        swModel.FeatureCurvePattern(3, 0.0254, 1, 0.00254, FalseFalseFalseFalseTrueFalseFalseFalse)

        'Access the curve-driven pattern feature
        status = swModelDocExt.SelectByID2("CrvPattern1""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swFeature = swSelectionMgr.GetSelectedObject6(1, -1)
        swCurveDrivenPatternFeatureData = swFeature.GetDefinition
        status = swCurveDrivenPatternFeatureData.AccessSelections(swModel, Nothing)
        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 = 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)
    End Sub
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
End Class

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

Subject:   Feedback on Help Topics
Page:   Create and Access Curve-driven Pattern Feature Example (VB.NET()
*   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:


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

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.