Create Revolve Features Example (VBA)

This example shows how to create revolve features.

'----------------------------------------------------------------------------
' Preconditions: Open a new part document.
'
' Postconditions: Two revolve features and one cut-revolve feature are created.
'----------------------------------------------------------------------------
Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swFeatMgr As SldWorks.FeatureManager
Dim swSelMgr As SldWorks.SelectionMgr
Dim boolstatus As Boolean

Sub main()

    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swModelDocExt = swModel.Extension
    Set swSelMgr = swModel.SelectionManager
   

    ' Create an axis
    boolstatus = swModelDocExt.SelectByID2("Right Plane", "PLANE", 0, 0, 0, True, 0, Nothing, swSelectOptionDefault)
    boolstatus = swModelDocExt.SelectByID2("Top Plane", "PLANE", 0, 0, 0, True, 0, Nothing, swSelectOptionDefault)
    swModel.InsertAxis2 True
   

    ' Create a rectangle
    boolstatus = swModelDocExt.SelectByID2("Top Plane", "PLANE", -0.08954836342753, 4.336873289503E-04, 0.006720765739942, False, 0, Nothing, swSelectOptionDefault)
    swModel.InsertSketch2 True
    swModel.ClearSelection2 True
    swModel.SketchRectangle -0.05668466821757, -0.02198379306525, 0, -0.01330857427717, 0.03972855876814, 0, 1
   

    ' Create the first revolve feature
    swModel.InsertSketch2 True
    swModel.ShowNamedView2 "*Trimetric", 8
  

    boolstatus = swModelDocExt.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)
    boolstatus = swModelDocExt.SelectByID2("Axis1", "AXIS", 0, 0, 0, True, 16, Nothing, swSelectOptionDefault)
    Set swFeatMgr = swModel.FeatureManager
  
    swFeatMgr.FeatureRevolve2 True, True, False, False, False, False, 0, 0, 6.28318530718, 0, False, False, 0.01, 0.01, 0, 0, 0, True, True, True
   

    ' Create a cut-revolve feature using a face on the revolve feature
    swSelMgr.EnableContourSelection = 0
    boolstatus = swModelDocExt.SelectByID2("", "FACE", -0.03095803920934, 0.01509536510872, 0.02198379306526, False, 0, Nothing, swSelectOptionDefault)
    swModel.InsertSketch2 True
    swModel.ClearSelection2 True
    swModel.SketchRectangle -0.04194874421597, 0.01774859621099, 0, -0.01883036471929, -0.01265654504095, 0, 1
    swModel.InsertSketch2 True
  

    boolstatus = swModelDocExt.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)
    boolstatus = swModelDocExt.SelectByID2("Line4@Sketch2", "EXTSKETCHSEGMENT", -0.01883036471929, 0.003802500010693, 0, True, 4, Nothing, swSelectOptionDefault)
    swFeatMgr.FeatureRevolveCut 6.26573201466, False, 0, 0, 0, 1, 1
   

    ' Create the second revolve feature using a face on the first revolve feature
    swSelMgr.EnableContourSelection = 0
    boolstatus = swModelDocExt.SelectByID2("", "FACE", -0.02333512246603, 0.03472018719853, 0.0219837930652, False, 0, Nothing, swSelectOptionDefault)
    swModel.InsertSketch2 True
    swModel.ClearSelection2 True
    swModel.CreateCircle2 -0.02232361399104, 0.03354683337932, 0, -0.01445073476016, 0.02795861773112, 0
    swModel.InsertSketch2 True
 

    boolstatus = swModelDocExt.SelectByID2("Sketch3", "SKETCH", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)
   

    boolstatus = swModelDocExt.SelectByRay(-1.81956067901865E-02, 1.80455411334037E-02, 2.17820530671702E-02, -0.400036026779312, -0.515038074910024, -0.758094294050284, 9.91972972972973E-04, 1, False, 4, 0)

    swFeatMgr.FeatureRevolve2 True, True, False, False, False, False, 0, 0, 6.28318530718, 0, False, False, 0.01, 0.01, 0, 0, 0, True, True, True
    swSelMgr.EnableContourSelection = 0

End Sub