Hide Table of Contents

Create Radiate Surface Feature Example (VBA)

This example shows how to create a radiate surface feature.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified document template exists.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Creates a new model document with a feature extrusion.
' 2. Creates Boss-Extrude1 and Surface-Radiate1 in the graphics area and
'    FeatureManager design tree.
' 3. Inspect the Immediate window.
'----------------------------------------------------------------------------

Dim swApp                As SldWorks.SldWorks
Dim Part                 As SldWorks.ModelDoc2
Dim swSelMgr             As SldWorks.SelectionMgr
Dim swSelData            As SldWorks.SelectData
Dim swRadiate            As SldWorks.SurfaceRadiateFeatureData
Dim swFeat               As SldWorks.Feature
Dim swEnt                As SldWorks.Entity
Dim vRadEnt              As Variant
Dim swRadDirEnt          As SldWorks.Entity
Dim i                    As Long
Dim boolStatus           As Boolean
Option Explicit

Sub main()

    Set swApp = Application.SldWorks
    Set Part = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2015\templates\Part.prtdot", 0, 0, 0)
    Set Part = swApp.ActiveDoc
   
    boolStatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -4.48901407839529E-02, 2.79954694016864E-02, 4.66820674117181E-03, False, 0, Nothing, 0)
    Part.SketchManager.InsertSketch True
    Part.ClearSelection2 True
    boolStatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstToRectEntity, swUserPreferenceOption_e.swDetailingNoOptionSpecified, False)
    boolStatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, swUserPreferenceOption_e.swDetailingNoOptionSpecified, True)
    Dim vSkLines As Variant
    vSkLines = Part.SketchManager.CreateCornerRectangle(-5.55749908365768E-02, 3.29075527136081E-02, 0, 4.78203409524033E-02, -3.17145296545045E-02, 0)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
    Part.ShowNamedView2 "*Trimetric", 8
    Part.SketchManager.InsertSketch True
    Part.ClearSelection2 True
    boolStatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 4, Nothing, 0)
   

    Dim myFeature As Object
    Set myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, False, 0, 0, 0.00254, 0.00254, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, True, True, True, 0, 0, False)
   

    boolStatus = Part.Extension.SelectByID2("", "EDGE", -4.47337592343047E-02, 3.28467250718631E-02, 2.58132540182032E-03, False, 2, Nothing, 0)
    boolStatus = Part.Extension.SelectByID2("", "EDGE", -5.56265649287866E-02, 1.56695101210289E-02, 2.5672149453726E-03, True, 2, Nothing, 0)
    boolStatus = Part.Extension.SelectByID2("", "EDGE", -1.40113588298618E-02, -3.17157034173761E-02, 2.54079743683633E-03, True, 2, Nothing, 0)
    boolStatus = Part.Extension.SelectByID2("", "EDGE", 0.047780958393389, -5.42256709667299E-03, 2.56078163948814E-03, True, 2, Nothing, 0)
    boolStatus = Part.Extension.SelectByID2("", "FACE", 4.78203409524554E-02, -3.05747564971171E-03, 5.46558985774936E-04, True, 1, Nothing, 0)
   

    Part.InsertRadiateSurface 0.0254, False, False
   

    Set swSelMgr = Part.SelectionManager
    Set swSelData = swSelMgr.CreateSelectData
   

    boolStatus = Part.Extension.SelectByID2("Surface-Radiate1", "REFSURFACE", 0, 0, 0, False, 0, Nothing, 0)
   

    Set swFeat = swSelMgr.GetSelectedObject6(1, -1)
    Set swRadiate = swFeat.GetDefinition
   

    ' Get radiate surface data
    Debug.Print "File = " & Part.GetPathName
    Debug.Print "  " & swFeat.Name
    Debug.Print "    Distance: " & swRadiate.Distance * 1000# & " mm"
    Debug.Print "    Flip? " & swRadiate.Flip
    Debug.Print "    Propagate to tangent faces? " & swRadiate.PropagateToTangentFaces

    ' Roll back to get direction reference and radiated edges
    boolStatus = swRadiate.AccessSelections(Part, Nothing)
    Set swRadDirEnt = swRadiate.DirectionReference
    Part.ClearSelection2 True

    vRadEnt = swRadiate.RadiatedEntities

    Debug.Print "Type as defined in swSelectType_e:"
    For i = 0 To swRadiate.GetRadiatedEntitiesCount - 1

        Set swEnt = vRadEnt(i)
        Debug.Print "  Radiated entity(" & i & ") = " & swEnt.GetType

    Next i

    swRadiate.ReleaseSelectionAccess

   
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 Radiate Surface Feature 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) 2015 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.