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Create Extruded Thin Feature Example (VBA)

This example shows how to create an extruded thin feature using a variety of parameter values.

'-----------------------------------------------------------------------------

' Preconditions: None.

'

' Postconditions: When the macro stops, press F5 five more times to create
' five different thin extrusion features.

'----------------------------------------------------------------------------

Option Explicit

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim myFeature As SldWorks.Feature
Dim swPart As SldWorks.PartDoc
Dim nStartCondition As Long
Dim nEndcondition1 As Long
Dim nEndcondition2 As Long
Dim lCase As Long
Dim dStartOffset As Double
Dim bFlipOffset As Boolean
Dim dThickness As Double
Dim swExtrusionData As SldWorks.ExtrudeFeatureData2
Dim lThinFeatureType As Long
Dim lCapEnds As Long
Dim bValue As Boolean

Dim boolstatus As Boolean

Option Explicit

Sub main()

    Set swApp = Application.SldWorks
   

    'New model document
    Dim swSheetWidth As Double
    swSheetWidth = 0
    Dim swSheetHeight As Double
    swSheetHeight = 0
    Set Part = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2018\templates\Part.prtdot", 0, swSheetWidth, swSheetHeight)
   

    Set swPart = Part
    Set Part = swApp.ActiveDoc
   

    'Set some parameters used for all cases
    nEndcondition1 = swEndCondBlind
    nEndcondition2 = swEndCondBlind
    dThickness = 0.001
    lThinFeatureType = 2 ' Mid-plane
    lCapEnds = 0

    'Create sketch
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -4.75777316877496E-02, 1.30140669704215E-02, 0.016264555537633, False, 0, Nothing, 0)
    Part.SketchManager.InsertSketch True
    Part.ClearSelection2 True

    Dim vSkLines As Variant
    vSkLines = Part.SketchManager.CreateCornerRectangle(-4.72149072628614E-02, 2.51029484316118E-02, 0, 6.72972660081509E-02, -4.56125914055245E-02, 0)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
   

    Part.ClearSelection2 True
   

    For lCase = 1 To 6

        Part.ClearSelection2 True
       

        bValue = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 4, Nothing, 0)
       

        Select Case lCase
            Case 1
                nStartCondition = swStartSketchPlane
                dStartOffset = 0#
                bFlipOffset = False
           

            Case 2
                nStartCondition = swStartOffset
                dStartOffset = 0#
                bFlipOffset = False
           

            Case 3
                nStartCondition = swStartOffset
                dStartOffset = 0#
                bFlipOffset = True
           

            Case 4
                nStartCondition = swStartOffset
                dStartOffset = 0.01
                bFlipOffset = False
           

            Case 5
                nStartCondition = swStartOffset
                dStartOffset = 0.01
                bFlipOffset = True
           

            Case 6
                nStartCondition = swStartVertex
                dStartOffset = 0#
                bFlipOffset = True
                dThickness = 0.01
           

            bValue = Part.Extension.SelectByID2("", "VERTEX", -0.05999251028807, 0.05489880658436, 0, True, 0, Nothing, 0)
           

        End Select
       

        Set myFeature = Part.FeatureManager.FeatureExtrusionThin2(True, False, False, nEndcondition1, nEndcondition2, 0.00254, 0.00254, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, True, dThickness, 0.00254, 0.00254, lThinFeatureType, lCapEnds, False, 0.005, True, True, nStartCondition, dStartOffset, bFlipOffset)
       

        Debug.Print myFeature.Name & " [" & myFeature.GetTypeName & "]"
       

        Set swExtrusionData = myFeature.GetDefinition
       

        bValue = swExtrusionData.AccessSelections(Part, Nothing)
       

        If (swExtrusionData.IsThinFeature = False) Then
            Debug.Print "ERROR: Must be a thin feature."
        End If
       

        Select Case swExtrusionData.FromType
       

            Case SwConst.swExtrudeFrom_e.swExtrudeFrom_SketchPlane
           

                Debug.Print "  from: sketchplane"
           

            Case SwConst.swExtrudeFrom_e.swExtrudeFrom_Offset
           

                Debug.Print "  from: offset"
           

                Debug.Print "    distance = " & swExtrusionData.FromOffsetDistance
                Debug.Print "    reverse  = " & swExtrusionData.FromOffsetReverse
           

            Case SwConst.swExtrudeFrom_e.swExtrudeFrom_SurfaceFacePlane
           

                Debug.Print "  from: surface"
           

            Case SwConst.swExtrudeFrom_e.swExtrudeFrom_Vertex
           

                Debug.Print "  from: vertex"
           

        End Select
       

        swExtrusionData.ReleaseSelectionAccess
       

        ' Examine the feature
        Stop
        ' Now delete the feature
        ' The sketch remains, so that you can select it again
        bValue = myFeature.Select2(True, 0)
       

        bValue = Part.Extension.DeleteSelection2(swDelete_Children)
   

    Next lCase

End Sub



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