Hide Table of Contents

Access Edges on Rip Feature Example (VBA)

This example shows how to access edges on a rip feature.

' Preconditions:
' 1. Verify that the specified model document exists.
' 2. Open an Immediate window.
' Postconditions:
' 1. Opens the specified part.
' 2. Creates Shell1 and Rip1 features.
' 3. Inspect the FeatureManager design tree, the graphics area, and
'    the Immediate window.
' NOTE: Because the model is used elsewhere, do not save changes.

Option Explicit

Sub main()

    Dim swApp                   As SldWorks.SldWorks
    Dim swModel                 As SldWorks.ModelDoc2
    Dim swSelMgr                As SldWorks.SelectionMgr
    Dim swFeat                  As SldWorks.Feature
    Dim swRip                   As SldWorks.RipFeatureData
    Dim vEdge                   As Variant
    Dim swEdge                  As SldWorks.Edge
    Dim swEnt                   As SldWorks.Entity
    Dim i                       As Long
    Dim lRipDirection           As Long
    Dim bRet                    As Boolean
    Dim longstatus As Long, longwarnings As Long


    Set swApp = Application.SldWorks

    lRipDirection = 64

    Set swModel = swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2017\tutorial\api\box.sldprt", 1, 0, "", longstatus, longwarnings)
    swApp.ActivateDoc2 "box", False, longstatus
    Set swModel = swApp.ActiveDoc
    Set swSelMgr = swModel.SelectionManager

    bRet = swModel.Extension.SelectByID2("", "FACE", -5.66885410894997E-02, 2.99999999999159E-02, 2.00993374069753E-02, False, 1, Nothing, 0)
    swModel.InsertFeatureShell 0.01, False

    bRet = swModel.Extension.SelectByID2("", "EDGE", 4.41585455038194E-02, 1.51990980971277E-02, 4.59121462268968E-02, True, lRipDirection, Nothing, 0)
    swModel.InsertRip 0.0001

    bRet = swModel.Extension.SelectByID2("Rip1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
    Set swFeat = swSelMgr.GetSelectedObject6(1, -1)

    ' Get rip feature data
    Set swRip = swFeat.GetDefinition

    Debug.Print "Gap: " & swRip.Gap * 1000# & " mm"

    bRet = swRip.AccessSelections(swModel, Nothing)

    Debug.Print "Number of edges: " & swRip.GetEdgesCount

    swModel.ClearSelection2 (True)

    vEdge = swRip.Edges

    For i = 0 To UBound(vEdge)

        Set swEdge = vEdge(i)
        Set swEnt = swEdge

        Debug.Print "Direction of rip for edge (0=current, 1=other, 2=both): " & swRip.GetDirection(swEdge)

        bRet = swEnt.Select4(True, Nothing)

    Next i


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

Subject:   Feedback on Help Topics
Page:   Access Edges on Rip Feature Example (VBA)
*   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:


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

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.