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.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