'================================================================

'Preconditions: Ensure that the specified part template exists.

'

'Postconditions:

'1. Base-Flange1 and Swept Flange1 are created.

'2. Inspect the graphics area and the FeatureManager design tree.

'================================================

Imports SolidWorks.Interop.sldworks

Imports SolidWorks.Interop.swconst

Imports System.Runtime.InteropServices

Imports System

 

Partial Class SolidWorksMacro

    Public Sub main()

 

        Dim swFeat As Feature

        Dim myFeature As Feature

        Dim swFeatMgr As FeatureManager

        Dim swFeatData As SweptFlangeFeatureData

        Dim customBendAllowanceData As CustomBendAllowance

        Dim swProfileSketch As Feature

        Dim skSegment As SketchSegment

        Dim Part As ModelDoc2

        Dim swPart As PartDoc

        Dim boolstatus As Boolean

        Dim longstatus As Integer

        Dim swSheetWidth As Double

        swSheetWidth = 0

        Dim swSheetHeight As Double

        swSheetHeight = 0

        Part = swApp.NewDocument("E:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\Tutorial\part.prtdot", 0, swSheetWidth, swSheetHeight)

 

        swPart = Part

        swApp.ActivateDoc2("Part1", False, longstatus)

        Part = swApp.ActiveDoc

 

        Part.SketchManager.InsertSketch(True)

        boolstatus = Part.Extension.SelectByID2("Front", "PLANE", -0.0350345417518034, 0.019677523162802, 0.00511863136830445, False, 0, Nothing, 0)

        Part.ClearSelection2(True)

        boolstatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstToRectEntity, swUserPreferenceOption_e.swDetailingNoOptionSpecified, False)

        boolstatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, swUserPreferenceOption_e.swDetailingNoOptionSpecified, True)

        Dim vSkLines As Object

        vSkLines = Part.SketchManager.CreateCornerRectangle(-0.0420403557341645, 0.0275066828701494, 0, 0.0475026757367474, -0.0220443628675665, 0)

        Part.ClearSelection2(True)

 

        Part.ShowNamedView2("*Trimetric", 8)

        Part.ViewZoomtofit2

 

        customBendAllowanceData = Part.FeatureManager.CreateCustomBendAllowance()

        customBendAllowanceData.KFactor = 0.5

 

        myFeature = Part.FeatureManager.InsertSheetMetalBaseFlange2(0.0007366, False, 0.0007366, 0.02, 0.01, False, 0, 0, 1, customBendAllowanceData, False, 0, 0.0001, 0.0001, 0.5, True, False, True, True)

 

        Part.ClearSelection2(True)

        Part.SketchManager.InsertSketch(True)

        boolstatus = Part.Extension.SelectByID2("", "FACE", 0.0441584745988735, 0.0275066828701256, -0.000252375262334681, True, 0, Nothing, 0)

 

        skSegment = Part.SketchManager.CreateLine(0.047503, 0#, 0#, 0.047503, -0.015713, 0#)

        Part.ClearSelection2(True)

        Part.SketchManager.InsertSketch(True)

 

        boolstatus = Part.Extension.SelectByID2("Sketch6", "SKETCH", 0.0254585357375204, -0.00378791126417555, -0.013876316631307, True, 0, Nothing, 0)

        boolstatus = Part.Extension.SelectByRay(0.0472949686339916, 0.0133307046879168, 0.000207707102561017, -0.499999999999997, -0.707106781186554, -0.499999999999995, 0.000423592175091009, 1, True, 0, 0)

        Part.ClearSelection2(True)

 

        'Select the sketch for the profile

        boolstatus = Part.Extension.SelectByID2("Sketch6", "SKETCH", 0.0254585357375204, -0.00378791126417555, -0.013876316631307, True, 0, Nothing, 0)

        swProfileSketch = Part.SelectionManager.GetSelectedObject6(1, -1)

        Part.ClearSelection2(True)

 

        'Select an edge for the path

        Dim swPathObj(0) As Edge

        boolstatus = Part.Extension.SelectByRay(0.0472949686339916, 0.0133307046879168, 0.000207707102561017, -0.499999999999997, -0.707106781186554, -0.499999999999995, 0.000423592175091009, 1, True, 0, 0)

        swPathObj(0) = Part.SelectionManager.GetSelectedObject6(1, -1)

 

        Part.ClearSelection2(True)

 

        swFeatMgr = Part.FeatureManager

 

        swFeatData = swFeatMgr.CreateDefinition(swFeatureNameID_e.swFmSweptFlange)

        swFeatData.EndOffset = 0

        swFeatData.FlangePosition = swSweptFlangePositionTypes_e.swSweptFlangePositionType_MaterialInside

        swFeatData.FlattenAlongPath = False

        swFeatData.OverrideDefaultSheetMetalParameters = False

        swFeatData.Path = swPathObj

        swFeatData.Profile = swProfileSketch

        swFeatData.ReverseDirection = False

        swFeatData.StartOffset = 0

        swFeatData.TrimSideBends = False

        swFeatData.UseDefaultBendAllowance = True

        swFeatData.UseDefaultBendRelief = True

        swFeatData.UseDefaultRadius = False

        swFeatData.UseGaugeTable = False

        swFeatData.UseMaterialSheetMetalParameters = False

        swFeat = swFeatMgr.CreateFeature(swFeatData)

        Part.ClearSelection2(True)

 

    End Sub

    ''' <summary>

    ''' The SldWorks swApp variable is pre-assigned for you.

    ''' </summary>

    Public swApp As SldWorks

End Class