Property UseGaugeTable As System.Boolean

Dim instance As ISketchedBendFeatureData
Dim value As System.Boolean
 
instance.UseGaugeTable = value
 
value = instance.UseGaugeTable

System.bool UseGaugeTable {get; set;}

property System.bool UseGaugeTable {
   System.bool get();
   void set ( &   System.bool value);
}

Property Value

'VBA
'==========================================================================
'This example demonstrates how to set the bend radius of a sketched bend
'by setting UseGaugeTable to false.
'
'Preconditions:
'1. Ensure the specified paths exist.
'2. Open an Immediate window.
'
'Postconditions:
'1. A part with Sheet-Metal, Base-Flange1, and Sketched Bend1 features is created.
'2. Inspect the Immediate window.
'=============================================================================

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim swPart As SldWorks.PartDoc
Dim myModelView As SldWorks.ModelView
Dim vSkLines As Variant
Dim swFeat As SldWorks.Feature
Dim swFeatMgr As SldWorks.FeatureManager
Dim customBendAllowanceData As SldWorks.CustomBendAllowance
Dim skSegment As SldWorks.SketchSegment
Dim CBAObject As SldWorks.CustomBendAllowance
Dim myFeature As SldWorks.Feature
Dim swFeatData As SldWorks.BaseFlangeFeatureData
Dim skBendFeatData As SldWorks.SketchedBendFeatureData
Dim myFeatData As SldWorks.SketchedBendFeatureData
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Dim swSheetWidth As Double
Dim swSheetHeight As Double
Option Explicit

Sub main()

    Set swApp = Application.SldWorks
   
    swSheetWidth = 0
    swSheetHeight = 0
    Set Part = swApp.NewDocument("D:\Program Files\SOLIDWORKS Corp\SOLIDWORKS (2)\DATA\Templates\Part.prtdot", 0, swSheetWidth, swSheetHeight)
 
    Set swPart = Part
    swApp.ActivateDoc2 "Part2", False, longstatus
    Set Part = swApp.ActiveDoc

    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -6.40395151030158E-02, 5.21578791231543E-02, 4.49083628119237E-03, False, 0, Nothing, 0)
    Part.SketchManager.InsertSketch True
    Part.ClearSelection2 True
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -2.96114446516235E-02, 3.44357811398094E-02, 0, 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)

    vSkLines = Part.SketchManager.CreateCornerRectangle(-5.22359192169088E-02, 3.27722168335384E-02, 0, 0.077854809533482, -4.14227512261475E-02, 0)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
   
    Part.ShowNamedView2 "*Trimetric", 8
    Part.ViewZoomtofit2
    Part.SketchManager.InsertSketch True
    Part.CloseFamilyTable
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Part.CloseFamilyTable

    Set customBendAllowanceData = Part.FeatureManager.CreateCustomBendAllowance()
   
    Set swFeatMgr = Part.FeatureManager

    Set swFeatData = swFeatMgr.CreateDefinition(swFeatureNameID_e.swFmBaseFlange)
    swFeatData.Initialize False, True, customBendAllowanceData, True, 1, True, 0.5, 0.0001, 0.0001
    swFeatData.BendRadius = 0.00635
    swFeatData.D1EndConditionDistance = 0.02
    swFeatData.D1EndConditionType = 1
    swFeatData.D1ReverseOffset = False
    swFeatData.D2EndConditionDistance = 0.01
    swFeatData.D2EndConditionType = 1
    swFeatData.D2ReverseOffset = False
    swFeatData.OffsetDirections = 1
    swFeatData.ReverseDirection = False
    swFeatData.ReverseThickness = False
    swFeatData.Thickness = 0.00531368
    swFeatData.UseGaugeTable = True
    swFeatData.GaugeTablePath = "D:\Program Files\SOLIDWORKS Corp\SOLIDWORKS (2)\lang\english\Sheet Metal Gauge Tables\bend allowance mm sample.xlsx"
    Set swFeat = swFeatMgr.CreateFeature(swFeatData)
    Part.ClearSelection2 True
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized

    Part.GraphicsRedraw2
    boolstatus = Part.Extension.SelectByRay(-1.81805886692246E-02, 2.58328472214089E-02, 0, -0.400036026779312, -0.515038074910024, -0.758094294050284, 1.07315913654528E-03, 2, False, 0, 0)
    Part.SketchManager.InsertSketch True
    Part.ClearSelection2 True
    boolstatus = Part.Extension.SelectByRay(-3.71158985098665E-02, 2.32231794094294E-02, 0, 0, 0, -1, 6.76279555664225E-04, 2, False, 0, 0)
    Part.ClearSelection2 True
   
    Set skSegment = Part.SketchManager.CreateLine(-0.007678, 0.057833, 0#, -0.059393, -0.042615, 0#)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
    Part.SketchManager.InsertSketch True
    boolstatus = Part.Extension.SelectByRay(-3.97811503331896E-03, 1.40228554924494E-02, 0, 0, 0, -1, 6.76279555664225E-04, 2, True, 0, 0)
   
    Set skBendFeatData = Part.FeatureManager.CreateDefinition(swFmSketchBend)
   
    skBendFeatData.BendAngle = 1.5707963267949
   
    'If using a default bend radius, you cannot set the bend radius
    skBendFeatData.UseDefaultBendRadius = False
    skBendFeatData.BendRadius = 0.001
    skBendFeatData.ReverseDirection = False
   
    'UseGaugeTable is valid only if UseDefaultBendRadius is false
    skBendFeatData.UseGaugeTable = True
   
    Set CBAObject = skBendFeatData.GetCustomBendAllowance()
    CBAObject.BendAllowance = 0.003
    Call skBendFeatData.SetCustomBendAllowance(CBAObject)
   
    Set myFeature = Part.FeatureManager.CreateFeature(skBendFeatData)
    Debug.Print "Sketched bend type name: " & myFeature.GetTypeName2()

    'Make some modifications
    Set myFeatData = myFeature.GetDefinition()
   
    'If using a gauge table, you cannot set the bend radius
    Debug.Print "Use gauge table? " & myFeatData.UseGaugeTable
   
    'Do not use gauge table, so you can set the bend radius
    myFeatData.UseGaugeTable = False
    myFeatData.BendRadius = 0.00635
   
    Debug.Print "Bend radius set to: " & myFeatData.BendRadius
   
    boolstatus = myFeature.ModifyDefinition(myFeatData, Part, Nothing)

End Sub

This property:

• is valid only if a gauge table is specified in a parent sheet metal feature (e.g., lofted bend, swept flange, base flange).
• is valid only if ISketchedBendFeatureData::UseDefaultBendRadius is set to false.
• is automatically set to false and cannot be changed if ISketchedBendFeatureData::UseDefaultBendRadius is set to true.
• must be set to false in order to set ISketchedBendFeatureData::BendRadius.