Hide Table of Contents

Create Revolve Features Example (VB.NET)

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.
'----------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System

Partial Class SolidWorksMacro

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


    Sub main()

        swModel = swApp.ActiveDoc
        swModelDocExt = swModel.Extension
        swSelMgr = swModel.SelectionManager

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

        
' Create a rectangle
        boolstatus = swModelDocExt.SelectByID2("Top Plane", "PLANE", -0.08954836342753, 0.0004336873289503, 0.006720765739942, False, 0, Nothing, swSelectOption_e.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, swSelectOption_e.swSelectOptionDefault)
        boolstatus = swModelDocExt.SelectByID2(
"Axis1", "AXIS", 0, 0, 0, True, 16, Nothing, swSelectOption_e.swSelectOptionDefault)
        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, swSelectOption_e.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, swSelectOption_e.swSelectOptionDefault)
        boolstatus = swModelDocExt.SelectByID2(
"Line4@Sketch2", "EXTSKETCHSEGMENT", -0.01883036471929, 0.003802500010693, 0, True, 4, Nothing, swSelectOption_e.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, swSelectOption_e.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, swSelectOption_e.swSelectOptionDefault)
        boolstatus = swModelDocExt.SelectByID2(
"", "EDGE", -0.02437300231541, 0.01770755773555, 0.02200276940169, True, 4, Nothing, swSelectOption_e.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

  
    
Public swApp As SldWorks


End Class

 


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 (VB.NET)
*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.