Select Multiple Sketch Segments for Sweep Path Example (VB.NET)
This example shows how to select multiple sketch segments for the path for a sweep feature.
'--------------------------------------------------------
' Preconditions: Verify that the part template exists.
'
' Postconditions:
' 1. Opens a new part.
' 2. Creates:
' * sketch of a circle.
' * sketch of a line.
' * another sketch of a line.
' 3. Selects the sketch of the circle for the sweep profile.
' 4. Selects the sketches of the lines for the sweep path
' and groups them as an object.
' 5. Creates a sweep feature.
' 6. Examine the FeatureManager design tree and graphics
' area.
'---------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Partial Class SolidWorksMacro
Public Sub main()
Dim swModel As ModelDoc2
Dim swModelDocExt As ModelDocExtension
Dim swSketchSegment As SketchSegment
Dim swSketchManager As SketchManager
Dim swFeatureManager As FeatureManager
Dim swFeature As Feature
Dim status As Boolean
swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2017\templates\Part.prtdot", 0, 0, 0)
swModelDocExt = swModel.Extension
swSketchManager = swModel.SketchManager
swFeatureManager = swModel.FeatureManager
'Create sketch of circle for the sweep profile
swSketchSegment = swSketchManager.CreateCircle(0.0#, 0.0#, 0.0#, 0.002394, -0.006333, 0.0#)
swSketchManager.InsertSketch(True)
'Create sketches of lines for the sweep path
status = swModelDocExt.SelectByID2("Right Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
swSketchManager.InsertSketch(True)
swSketchSegment = swSketchManager.CreateLine(-0.0#, 0.0#, 0.0#, 0.088481, 0.035691, 0.0#)
swSketchManager.InsertSketch(True)
swModel.ClearSelection2(True)
status = swModelDocExt.SelectByID2("Right Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
swSketchManager.InsertSketch(True)
swSketchSegment = swSketchManager.CreateLine(0.088481, 0.035691, 0.0#, 0.079214, 0.076295, 0.0#)
swSketchManager.InsertSketch(True)
swModel.ClearSelection2(True)
'Select the sketch of the circle for the sweep profile
status = swModelDocExt.SelectByID2("Sketch1", "SKETCH", -0.00586834883582351, -0.00337646707201764, 0, False, 1, Nothing, 0)
'Select the sketches of the lines for the sweep path and group them as an object
status = swModelDocExt.SelectByID2("Line1@Sketch2", "EXTSKETCHSEGMENT", 0.0379259971310087, 0.0152983890733924, 0, True, 4, Nothing, 0)
status = swModelDocExt.SelectByID2("Line1@Sketch3", "EXTSKETCHSEGMENT", 0.0848435978763939, 0.0516285284155501, 0, True, 4, Nothing, 0)
status = swModelDocExt.SelectByID2("Unknown", "SELOBJGROUP", 0, 0, 0, True, 4, Nothing, 0)
'Create the sweep feature
swFeature = swFeatureManager.InsertProtrusionSwept4(False, False, 0, False, False, 0, 0, False, 0, 0, 0, 0, True, True, True, 0, True, False, 0, 0)
End Sub
''' <summary>
''' The SldWorks swApp variable is pre-assigned for you.
''' </summary>
Public swApp As SldWorks
End Class