Create and Edit Circular Sketch Pattern Example (VBA)

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.
'------------------------------------------------------------
Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSketchMgr As SldWorks.SketchManager
Dim swSketchSegment As SldWorks.SketchSegment
Dim vSkLines As Variant
Dim boolstatus As Boolean
Dim longstatus As Long

Sub main()

    Set swApp = Application.SldWorks    

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

    ' Create part document
    Set swModel = swApp.NewDocument("C:\Documents and Settings\All Users\Application Data\SOLIDWORKS\SOLIDWORKS 2014\templates\Part.prtdot", 0, 0, 0)
    swApp.ActivateDoc2 "Part1", False, longstatus
    Set swModel = swApp.ActiveDoc
    Set swSketchMgr = swModel.SketchManager
    Set swModelDocExt = swModel.Extension    

    ' Sketch a circle
    Set swSketchSegment = swSketchMgr.CreateCircle(0#, 0#, 0#, 0.045549, 0.013926, 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