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Insert Swept-surface Feature Example (VBA)

This example shows how to create a swept-surface feature.

'---------------------------------------------------------------------------
' Preconditions: Verify that the part template exists.
'
' Postconditions:
' 1. Opens a new part.
' 2. Creates two sketches.
' 3. Inserts a swept-surface feature.
' 4. Examine the FeatureManager design tree and
'    graphics area.
'---------------------------------------------------------------------------
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSketchManager As SldWorks.SketchManager
Dim swSketchSegment As SldWorks.SketchSegment
Dim swPathFeat As SldWorks.Feature
Dim swFeatureMgr As SldWorks.FeatureManager
Dim swSweep As SldWorks.SweepFeatureData
Dim status As Boolean
Sub main()
    Set swApp = Application.SldWorks    
    'Open new part document
    Set swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2018\templates\part.prtdot", 0, 0, 0)
    Set swModelDocExt = swModel.Extension    
    'Create a sketch
    Set swSketchManager = swModel.SketchManager
    swSketchManager.InsertSketch True
    status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    Set swSketchSegment = swSketchManager.CreateLine(0#, 0#, 0#, 0.068491, 0.049604, 0#)
    Set swSketchSegment = swSketchManager.CreateLine(0.068491, 0.049604, 0#, 0.10923, 0.112837, 0#)
    Set swSketchSegment = swSketchManager.CreateLine(0.10923, 0.112837, 0#, 0.194652, 0.154023, 0#)
    swSketchManager.InsertSketch True    
    swModel.ViewZoomtofit2
    swModel.ShowNamedView2 "*Isometric", 7
    swModel.ClearSelection2 True
    'Create another sketch
    status = swModelDocExt.SelectByID2("Right Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    swSketchManager.InsertSketch True
    Set swSketchSegment = swSketchManager.CreateLine(-0#, 0#, 0#, 0.021042, 0.091756, 0#)
    Set swSketchSegment = swSketchManager.CreateLine(0.021042, 0.091756, 0#, 0.098366, 0.085093, 0#)
    Set swSketchSegment = swSketchManager.CreateLine(0.098366, 0.085093, 0#, 0.143062, 0.122696, 0#)
    swModel.ClearSelection2 True
    swSketchManager.InsertSketch True    
    'Insert surface sweep
    status = swModelDocExt.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, True, 4, Nothing, 0)
    

    Set swFeatureMgr = swModel.FeatureManager

    Set swSweep = swFeatureMgr.CreateDefinition(swFmRefSurface)

    swSweep.TangentPropagation = False
    swSweep.TwistControlType = 0
    swSweep.MaintainTangency = False
    swSweep.AdvancedSmoothing = False
    swSweep.StartTangencyType = 0
    swSweep.EndTangencyType = 0
    swSweep.PathAlignmentType = 0
    swSweep.FeatureScope = True
    swSweep.AutoSelect = True
    swSweep.SetTwistAngle 0#
    swSweep.MergeSmoothFaces = True
    swSweep.CircularProfile = False
    swSweep.CircularProfileDiameter = 0#
    swSweep.Direction = 0
   

    Set swPathFeat = swFeatureMgr.CreateFeature(swSweep)
 

End Sub


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