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Get Rib Feature Data Example (VBA)

This example shows how to get rib feature data.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified model document exists.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Opens the part document.
' 2. Creates Shell1, Plane1, and Rib1.
' 3. Inspect the FeatureManager design tree, the graphics area, and the
'    Immediate window.
'
' NOTE: Because the model is used elsewhere, do not save changes.
'---------------------------------------------------------------------------
Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim myRefPlane As SldWorks.RefPlane
Dim skSegment As SldWorks.SketchSegment
Dim swSelMgr As SldWorks.SelectionMgr
Dim swFeat As SldWorks.Feature
Dim swRibFeat As SldWorks.RibFeatureData2
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Option Explicit
Sub main()

    Set swApp = Application.SldWorks

    Set Part = swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2017\tutorial\api\block20.sldprt", 1, 0, "", longstatus, longwarnings)
    swApp.ActivateDoc2 "block20", False, longstatus
    Set Part = swApp.ActiveDoc
   

    boolstatus = Part.Extension.SelectByID2("", "FACE", -8.78816842651986E-03, 3.96239999998897E-02, -2.92468281514857E-02, False, 1, Nothing, 0)
    Part.InsertFeatureShell 0.00254, False
   

    boolstatus = Part.Extension.SelectByID2("", "FACE", 2.64031138414111E-03, 0.028407059059532, -6.13970439424634E-02, True, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("", "FACE", -0.059937899786064, 2.77866864457792E-02, -8.77977980189826E-03, True, 1, Nothing, 0)
   

    Set myRefPlane = Part.FeatureManager.InsertRefPlane(128, 0, 128, 0, 0, 0)
    Part.ClearSelection2 True
   

    boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", 6.64896553058725E-03, 0.109417877974863, 5.24178648701081E-02, False, 0, Nothing, 0)
    Part.SketchManager.InsertSketch True

    Set skSegment = Part.SketchManager.CreateLine(-0.085797, 0.021082, 0#, -0.03423, 0.035134, 0#)
    Set skSegment = Part.SketchManager.CreateLine(-0.03423, 0.035134, 0#, 0.007726, 0.025357, 0#)
    Set skSegment = Part.SketchManager.CreateLine(0.007726, 0.025357, 0#, 0.111514, 0.039624, 0#)
    Part.ClearSelection2 True

    Part.SketchManager.InsertSketch True
    Part.ClearSelection2 True
    boolstatus = Part.Extension.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)
    Part.FeatureManager.InsertRib True, False, 0.00254, 0, False, False, True, 1.74532925199433E-02, False, False
   

    Set swSelMgr = Part.SelectionManager
    Set swFeat = swSelMgr.GetSelectedObject6(1, -1)
    Set swRibFeat = swFeat.GetDefinition

    Debug.Print "Rib feature type as defined in swRibType_e: " & swRibFeat.Type
    Debug.Print "Thickness: " & swRibFeat.Thickness
    Debug.Print "Extrusion direction as defined in swRibExtrusionDirection_e: " & swRibFeat.ExtrusionDirection
    Debug.Print "Rib has a draft? " & swRibFeat.EnableDraft
    If swRibFeat.EnableDraft Then
        Debug.Print "    Draft angle: " & swRibFeat.DraftAngle
        Debug.Print "    Draft outward? " & swRibFeat.DraftOutward
    End If
    Debug.Print "Add material to reverse side of the rib? " & swRibFeat.FlipSide
    Debug.Print "Rib is extruded on two sides of the midplane? " & swRibFeat.IsTwoSided
    If Not swRibFeat.IsTwoSided Then
        Debug.Print "Single-sided rib is extruded on the reverse side? " & swRibFeat.ReverseThicknessDir
    End If
  

End Sub

 



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