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Create Extruded Thin Feature Example (VBA)

This example shows how to create an extruded thin feature.

 

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

'

' Preconditions: Model document with a sketch named Sketch2 is open.

'

' Postconditions: None

'

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

Option Explicit

Dim swApp As SldWorks.SldWorks

Sub main()

    Dim swModel           As SldWorks.ModelDoc2

    Dim bValue            As Boolean

    Dim swFeature         As SldWorks.Feature

    Dim nStartCondition   As SwConst.swStartConditions_e

    Dim nEndcondition1    As SwConst.swEndConditions_e

    Dim nEndcondition2    As SwConst.swEndConditions_e

    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

    

    

    

    ' Connect to SOLIDWORKS

    Set swApp = Application.SldWorks

    ' Get active document

    Set swModel = swApp.ActiveDoc

    ' Set some parameters used for all cases

    nEndcondition1 = swEndCondBlind

    nEndcondition2 = swEndCondBlind

    dThickness = 0.01

    lThinFeatureType = 2 ' Mid-plane

    lCapEnds = 0

    

    For lCase = 1 To 7

    

        swModel.ClearSelection2 True

        

        bValue = swModel.Extension.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 0, 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 = swStartSurface

                dStartOffset = 0#

                bFlipOffset = True

                dThickness = 0.005

                

                bValue = swModel.Extension.SelectByID2("", "FACE", -0.0227247722911, 0.01533611968841, 0, True, 0, Nothing, 0)

        

            Case 7            

                nStartCondition = swStartVertex

                dStartOffset = 0#

                bFlipOffset = True

                dThickness = 0.005

                

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

                

        End Select

        

        Set swFeature = swModel.FeatureManager.FeatureExtrusionThin2(True, False, False, nEndcondition1, nEndcondition2, 0.03, 0.03, False, False, False, False, 0#, 0#, False, False, False, False, False, dThickness, 0#, 0#, lThinFeatureType, lCapEnds, False, 0.005, True, True, nStartCondition, dStartOffset, bFlipOffset)

        

        

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

        

        Set swExtrusionData = swFeature.GetDefinition

        

        bValue = swExtrusionData.AccessSelections(swModel, 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 = swFeature.Select2(True, 0)

        

        bValue = swModel.Extension.DeleteSelection2(swDelete_Children)

               

    Next lCase

        

End Sub



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