Extend Sketch Entity Example (VB.NET)
This example shows how to extend a selected sketch entity (e.g., line,
segment, or arc) to meet another sketch entity.
'-------------------------------------------------------------------
' Preconditions: Open a new part document.
'
' Postconditions:
' 1. Inserts a new sketch is inserted.
' 2. Creates two non-parallel lines.
' 3. Extends the first line to meet the second line.
' 4. Examine the graphics area.
'-------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Partial Class SolidWorksMacro
Dim swModel As ModelDoc2
Dim swModelDocExt As ModelDocExtension
Dim swSketchMgr As SketchManager
Dim boolstatus As Boolean
Sub main()
swModel = swApp.ActiveDoc
swModelDocExt = swModel.Extension
swSketchMgr = swModel.SketchManager
swSketchMgr.InsertSketch(False)
' Create two non-parallel lines
swSketchMgr.CreateLine(-0.5,
0.88, 0.0#, -0.21, -0.13, 0.0#)
swSketchMgr.CreateLine(-0.75, -1.128, 0.0#, 0.41, -1.128,
0.0#)
swModel.ViewZoomtofit2
' Set the selection mode to default
swModel.SetPickMode()
' Select the sketch line to extend
boolstatus = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT",
0.0#, 0.0#, 0.0#, False,
0, Nothing,
0)
' Extend the selected sketch line
to meet the second line
boolstatus = swSketchMgr.SketchExtend(0.0#,
0.0#, 0.0#)
swSketchMgr.InsertSketch(True)
End Sub
Public swApp As SldWorks
End Class