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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:\Documents and Settings\All Users\Application Data\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.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)



        ' Close the sketch and rebuild



        ' 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)



        ' 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_")




    End Sub


    ''' <summary>

    ''' The SldWorks swApp variable is pre-assigned for you.

    ''' </summary>

    Public swApp As SldWorks


End Class

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