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Get Guide Curves in Sweep Feature Example (VB.NET)

This example shows how to get the guide curves in a sweep feature.

'----------------------------------------
' Preconditions:
' 1. Verify that the specified part document
'    template exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Creates a new part document.
' 2. Creates a sweep feature.
' 3. Prints to the Immediate window the
'    number of guide curves in the sweep
'    feature.
' 4. Accesses the guide curves in the sweep feature.
' 5. Prints to the Immediate window the feature types
'    of the guide curves.
' 6. Releases access to the sweep feature.
' 7. Examine the Immediate window.
'----------------------------------------

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 swFeature As Feature
        Dim swFeatureMgr As FeatureManager
        Dim swSweepFeatureData As SweepFeatureData
        Dim pointArray As Object
        Dim points() As Double
        Dim guideCurves As Object
        Dim guideCurve As Object
        Dim nbrGuideCurves As Long
        Dim status As Boolean
        Dim i As Long
 
        'Create new model document
        swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SolidWorks 2015\templates\Part.prtdot", 0, 0, 0)
        swModelDocExt = swModel.Extension
 
        'Sketch an ellipse for sweep profile
        swModel.ClearSelection2(True)
        swSketchMgr = swModel.SketchManager
        status = swModelDocExt.SelectByID2("Top Plane""PLANE", 0, 0, 0, False, 0, Nothing, 0)
        swSketchMgr.InsertSketch(True)
        swSketchSegment = swSketchMgr.CreateEllipse(0, 0, 0, -0.064925207354862, 0, 0, 0, -0.0360377802938881, 0)
        swModel.ClearSelection2(True)
        swSketchMgr.InsertSketch(True)
 
        'Sketch a line for sweep path
        status = swModelDocExt.SelectByID2("Front Plane""PLANE", 0, 0, 0, False, 0, Nothing, 0)
        swSketchMgr.InsertSketch(True)
        swSketchSegment = swSketchMgr.CreateLine(0.0#, 0.0#, 0.0#, 0.0#, 0.059816, 0.0#)
        swModel.ClearSelection2(True)
        swSketchMgr.InsertSketch(True)
 
        'Sketch a spline for sweep guide curve
        status = swModelDocExt.SelectByID2("Front Plane""PLANE", 0, 0, 0, False, 0, Nothing, 0)
        swSketchMgr.InsertSketch(True)
        ReDim points(5)
        points(0) = -0.064925207354862
        points(1) = 0
        points(2) = 0
        points(3) = -0.00576005360247873
        points(4) = 0.0595205538922803
        points(5) = 0
        pointArray = points
        swSketchSegment = swSketchMgr.CreateSpline((pointArray))
        swModel.ClearSelection2(True)
        status = swModelDocExt.SelectByID2("Unknown""MANIPULATOR", -0.0481685228359519, 0.0168573405240843, 0, False, 0, Nothing, 0)
        swModel.ClearSelection2(True)
        swSketchMgr.InsertSketch(True)
        swModel.ViewZoomtofit2()
 
        'Select the profile, path, and guide curve
        status = swModelDocExt.SelectByID2("Sketch1""SKETCH", 0, 0, 0, True, 0, Nothing, 0)
        status = swModelDocExt.SelectByID2("Sketch2""SKETCH", 0, 0, 0, True, 0, Nothing, 0)
        status = swModelDocExt.SelectByID2("Sketch3""SKETCH", 0, 0, 0, True, 0, Nothing, 0)
        swModel.ClearSelection2(True)
        status = swModelDocExt.SelectByID2("Sketch1""SKETCH", 0, 0, 0, False, 1, Nothing, 0)
        status = swModelDocExt.SelectByID2("Sketch2""SKETCH", 0, 0, 0, True, 4, Nothing, 0)
        status = swModelDocExt.SelectByID2("Sketch3""SKETCH", 0, 0, 0, True, 2, Nothing, 0)
 
        'Create the sweep feature
        swFeatureMgr = swModel.FeatureManager
        swFeature = swFeatureMgr.InsertProtrusionSwept3(FalseFalse, swTwistControlType_e.swTwistControlFollowPath, FalseFalse, swTangencyType_e.swTangencyNone, swTangencyType_e.swTangencyNone, False, 0, 0, swThinWallType_e.swThinWallOneDirection, 0, TrueTrueTrue, 0, True)
        Debug.Print("Feature type: " & swFeature.GetTypeName2)
 
        'Change the orientation of the view
        swModel.ShowNamedView2("*Isometric", 7)
 
        'Access sweep feature data, get guide curves,
        'get feature type of guide curves, and release
        'access to sweep feature
        swSweepFeatureData = swFeature.GetDefinition
        nbrGuideCurves = swSweepFeatureData.GetGuideCurvesCount
        Debug.Print("  Number of guide curves: " & nbrGuideCurves)
        status = swSweepFeatureData.AccessSelections(swModel, Nothing)
        Debug.Print("    Guide curve: ")
        guideCurves = swSweepFeatureData.GuideCurves
        For i = 0 To (nbrGuideCurves - 1)
            guideCurve = guideCurves(i)
            Debug.Print("      Type of feature: " & swSweepFeatureData.GetGuideCurvesType(i))
        Next i
        swSweepFeatureData.ReleaseSelectionAccess()
 
    End Sub
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
 
 
End Class 


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