Get Properties of Sketch Pattern Feature Example (VB.NET)

This example shows how to get the properties of a sketch pattern feature.

'----------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified document exists.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Creates Boss-Extrude2, Sketch3, and Sketch-Pattern1.
' 2. Inspect the Immediate window.
'
' NOTE: Because the model 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
 
    Dim Part As ModelDoc2
    Dim myFeature As Feature
    Dim swSketchPatt As SketchPatternFeatureData
    Dim vBasePt As Object
    Dim skPoint As Object
    Dim vSkLines As Object
    Dim swSketch As Sketch
    Dim swSketchFeat As Feature
    Dim swPatternTransform As MathTransform
    Dim boolstatus As Boolean
    Dim i As Integer
    Dim longstatus As Integer
    Dim longwarnings As Integer
 
    Sub main()
 
        Part = swApp.OpenDoc6("C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\api\block20.sldprt", 1, 0, "", longstatus, longwarnings)
        swApp.ActivateDoc2("block20", False, longstatus)
 
        boolstatus = Part.Extension.SelectByID2("", "FACE", -0.0407921768468213, 0.0396239999998329, -0.0402814031592129, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstToRectEntity, swUserPreferenceOption_e.swDetailingNoOptionSpecified, False)
        boolstatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, swUserPreferenceOption_e.swDetailingNoOptionSpecified, True)
        vSkLines = Part.SketchManager.CreateCornerRectangle(-0.0518589252521906, 0.0451811131877662, 0, -0.0357471289475484, 0.0286242963995278, 0)
        Part.SketchManager.InsertSketch(True)
 
        boolstatus = Part.Extension.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 4, Nothing, 0)
        myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, False, 0, 0, 0.00254, 0.00254, False, False, False, False, 0.0174532925199433, 0.0174532925199433, False, False, False, False, True, True, True, 0, 0, False)
 
        Part.SketchManager.InsertSketch(True)
        boolstatus = Part.Extension.SelectByID2("", "FACE", -0.00770328176440671, 0.0396239999998897, -0.00762437790422155, False, 0, Nothing, 0)
        skPoint = Part.SketchManager.CreatePoint(-0.00527, 0.051345, 0.0#)
        skPoint = Part.SketchManager.CreatePoint(-0.005854, 0.025783, 0.0#)
        skPoint = Part.SketchManager.CreatePoint(-0.005888, -0.000009, 0.0#)
        skPoint = Part.SketchManager.CreatePoint(0.019408, 0.051285, 0.0#)
        skPoint = Part.SketchManager.CreatePoint(0.019093, 0.024628, 0.0#)
        skPoint = Part.SketchManager.CreatePoint(0.019629, -0.000148, 0.0#)
        skPoint = Part.SketchManager.CreatePoint(0.043756, 0.051962, 0.0#)
        skPoint = Part.SketchManager.CreatePoint(0.043146, 0.025865, 0.0#)
        skPoint = Part.SketchManager.CreatePoint(0.043401, 0.000225, 0.0#)
        Part.ClearSelection2(True)
        Part.SketchManager.InsertSketch(True)
 
        boolstatus = Part.Extension.SelectByID2("Boss-Extrude2", "BODYFEATURE", -0.0477922378944982, 0.0421639999998433, 0.0233214950450815, False, 4, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("Sketch3", "SKETCH", 0, 0, 0, True, 64, Nothing, 0)
 
        swSketchFeat = Part.FeatureManager.FeatureSketchDrivenPattern(True, False)
        swSketchPatt = swSketchFeat.GetDefinition
 
        swSketchPatt.AccessSelections(Part, Nothing)
 
        swSketch = swSketchPatt.Sketch
        i = swSketch.GetSketchPointsCount2
 
        swPatternTransform = swSketchPatt.GetTransform(i)
 
        vBasePt = swSketchPatt.GetBasePoint
 
        Debug.Print(swSketchFeat.Name)
        Debug.Print("  Create pattern using only geometry? " & swSketchPatt.GeometryPattern)
        Debug.Print("  Pattern seed coordinates in mm:  (" & vBasePt(0) * 1000.0# & ", " & vBasePt(1) * 1000.0# & ", " & vBasePt(2) * 1000.0# & ")")
        Debug.Print("  Body count: " & swSketchPatt.GetPatternBodyCount)
        Debug.Print("  Face count: " & swSketchPatt.GetPatternFaceCount)
        Debug.Print("  Feature count: " & swSketchPatt.GetPatternFeatureCount)
        Debug.Print("  Reference point type (-1 for centroid): " & swSketchPatt.GetReferencePointType)
        Debug.Print("  Use centroid as the reference point? " & swSketchPatt.UseCentroid)
        Debug.Print("  Propagate visual properties? " & swSketchPatt.PropagateVisualProperty)
 
        swSketchPatt.ReleaseSelectionAccess()
 
    End Sub
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
 
 
End Class