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Get Rib Feature Data Example (VB.NET)

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 Shell1Plane1, 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.

Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
Partial Class SolidWorksMacro
    Dim Part As ModelDoc2
    Dim myRefPlane As RefPlane
    Dim skSegment As SketchSegment
    Dim swSelMgr As SelectionMgr
    Dim swFeat As Feature
    Dim swRibFeat As RibFeatureData2
    Dim boolstatus As Boolean
    Dim longstatus As Integer, longwarnings As Integer
    Sub main()
        Part = swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2017\tutorial\api\block20.sldprt", 1, 0, "", longstatus, longwarnings)
        swApp.ActivateDoc2("block20"False, longstatus)
        Part = swApp.ActiveDoc
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.00878816842651986, 0.0396239999998897, -0.0292468281514857, False, 1, Nothing, 0)
        Part.InsertFeatureShell(0.00254, False)
        boolstatus = Part.Extension.SelectByID2("""FACE", 0.00264031138414111, 0.028407059059532, -0.0613970439424634, True, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.059937899786064, 0.0277866864457792, -0.00877977980189826, True, 1, Nothing, 0)
        myRefPlane = Part.FeatureManager.InsertRefPlane(128, 0, 128, 0, 0, 0)
        boolstatus = Part.Extension.SelectByID2("Plane1""PLANE", 0.00664896553058725, 0.109417877974863, 0.0524178648701081, False, 0, Nothing, 0)
        skSegment = Part.SketchManager.CreateLine(-0.085797, 0.021082, 0.0#, -0.03423, 0.035134, 0.0#)
        skSegment = Part.SketchManager.CreateLine(-0.03423, 0.035134, 0.0#, 0.007726, 0.025357, 0.0#)
        skSegment = Part.SketchManager.CreateLine(0.007726, 0.025357, 0.0#, 0.111514, 0.039624, 0.0#)
        boolstatus = Part.Extension.SelectByID2("Sketch2""SKETCH", 0, 0, 0, False, 0, Nothing, 0)
        Part.FeatureManager.InsertRib(TrueFalse, 0.00254, 0, FalseFalseTrue, 0.0174532925199433, FalseFalse)
        swSelMgr = Part.SelectionManager
        swFeat = swSelMgr.GetSelectedObject6(1, -1)
        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
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
End Class



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