Create and Edit Circular Sketch Pattern Example (VB.NET)

This example shows how to create and edit a circular sketch pattern.

'------------------------------------------------------------
' Preconditions: Verify that the specified part document template
' exists.
'
' Postconditions:
' 1. Opens a new part document and creates a sketch.
' 2. Inserts a circular sketch pattern of four instances.
' 3. Closes the sketch.
' 4. Opens the circular sketch pattern for editing.
' 5. Deletes an instance of circular sketch pattern, leaving
'    three instances.
' 6. Examine the graphics area.
'------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System

Partial Class SolidWorksMacro

    Public Sub main()

        Dim swModel As ModelDoc2
        Dim swModelDocExt As ModelDocExtension
        Dim swSketchMgr As SketchManager
        Dim swSketchSegment As SketchSegment
        Dim vSkLines As Object
        Dim boolstatus As Boolean
        Dim longstatus As Long

        ' Reset the counts for untitled documents for this macro
        swApp.ResetUntitledCount(0, 0, 0)

        ' Create and activate a part document
        swModel = swApp.NewDocument("C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2008\templates\Part.prtdot", 0, 0, 0)
        swApp.ActivateDoc2("Part1", False, longstatus)
        swModel = swApp.ActiveDoc

        swSketchMgr = swModel.SketchManager
        swModelDocExt = swModel.Extension

        ' Sketch a circle
        swSketchSegment = swSketchMgr.CreateCircle(0.0#, 0.0#, 0.0#, 0.045549, 0.013926, 0.0#)

        ' Clear any selections and change
        ' the view orientation to Front
        swModel.ClearSelection2(True)
        swModel.ShowNamedView2("*Front", 1)

        ' Create a rectangle
        vSkLines = swSketchMgr.CreateCornerRectangle(-0.005867589431389, 0.03694408160504, 0, 0.004563680668858, 0.02673012963188, 0)

        ' Create a circular sketch pattern
        ' using the rectangle
        boolstatus = swSketchMgr.CreateCircularSketchStepAndRepeat(0.03184378021964, 4.732863934409, 4, 1.570796326795, True, "", True, True, True)
        swModel.ClearSelection2(True)

        ' Close the sketch and rebuild
        swSketchMgr.InsertSketch(True)

        ' Select an entity in the circular sketch pattern
        ' and open the circular sketch pattern to edit it
        boolstatus = swModelDocExt.SelectByID2("Line1@Sketch1", "EXTSKETCHSEGMENT", -0.002390499397973, 0.03694408160504, 0, False, 0, Nothing, 0)
        swModel.EditSketch()

        ' Delete an instance of the circular
        ' sketch pattern and close the sketch
        boolstatus = swSketchMgr.EditCircularSketchStepAndRepeat(0.03184378021964, 4.732863934409, 3, 1.570796326795, True, "", True, True, True, "Line2_Line1_Line4_Line3_")
        swModel.ClearSelection2(True)
        swSketchMgr.InsertSketch(True)

    End Sub

    ''' <summary>

    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks

End Class