Hide Table of Contents

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.SelectByID2("", "EDGE", -0.02437300231541, 0.01770755773555, 0.02200276940169, True, 4, Nothing, swSelectOptionDefault)
    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



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Create Revolve Features Example (VBA)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2017 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.