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Create and Edit Circular Sketch Pattern Example (VBA)

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

 

' ******************************************************************************

'

' Preconditions:

'       (1) SolidWorks is running.

'       (2) The part template exists in the specified folder.

'

' Postconditions:

'         (1) A sketch is created.

'         (2) A circular sketch pattern is created in the open sketch.

'         (3) Sketch is closed.

'         (4) Circular sketch pattern is opened for editing.

'         (5) Circular sketch pattern is edited -- an instance of

'             the circular sketch pattern is deleted.

'

' ******************************************************************************

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 2010\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



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