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Insert Sheet Metal Gusset Feature Example (VB.NET)

This example shows how to insert a sheet metal gusset feature and modify its data.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Open install_dir\samples\tutorial\api\SMGussetAPI.sldprt.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Inserts four sheet metal gussets.
' 2. Press F5 repeatedly and observe the gusset modifications.
' 3. Inspect the Immediate window for the flatten settings of all gussets.
' 4. Expand Flat-Pattern in the FeatureManager design tree, right-click 
'    Flat-Pattern(1), and click Unsuppress.
' 5. Observe the center marks and profiles of all the gussets in their
'    flattened states.
'
' 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 myFeature As Feature
    Dim myFeature1 As Feature
    Dim myFeature2 As Feature
    Dim myFeature3 As Feature
    Dim swFeat As Feature
    Dim swFeatData As SMGussetFeatureData
    Dim boolstatus As Boolean
 
    Sub main()
 
        Part = swApp.ActiveDoc
 
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0538403893476698, 0.0036701308754914, 0.05530817474488, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0177780871801474, -0.0307393226379986, 0.0341128529187245, True, 0, Nothing, 0)
 
        ' Gusset #1 insertion parameters
        '1.  bOffset                    = True
        '2.  dOffset                    = 50 mm
        '3.  bFlipOffsetSide            = False
        '4.  profDimType                = 0 (indent depth dimensioning scheme)
        '5.  dIndentDepth               = 10 mm
        '6.  dLength                    = 0
        '7.  bUseAngle                  = False
        '8.  dHeight                    = 0
        '9   dAngle                     = 0
        '10. bFlipSides                 = False
        '11. dWidth                     = 10 mm
        '12. dThickness                 = 3 mm
        '13. bDraft                     = True
        '14. dDraftAngle                = 3 degrees
        '15. bInnerCornerFillet         = True
        '16. dInnerCornerFilletRadius   = 2 mm
        '17. bOuterCornerFillet         = True
        '18. dOuterCornerFilletRadius   = 1 mm
        '19. gussetType                 = 0 (rounded back)
        '20  bEdgeFillet                = False
        '21. dEdgeFilletRadius          = 0 mm
        '22. bOverrideDoc               = True
        '23. bShowProfile               = True
        '24. bShowCenter                = True
 
        myFeature = Part.FeatureManager.InsertSheetMetalGussetFeature3(True, 0.05, False, swSheetMetalGussetProfileDimType_e.swSheetMetalGussetProfileDimType_IndentDepth, 0.01, 0, False, 0, 0, True, 0.01, 0.003, True, 3 * 0.0175, True, 0.002, True, 0.001, swSheetMetalRibGussetType_e.swSheetMetalRibGussetType_Rounded, False, 0, TrueTrueTrue)
        Part.ClearSelection2(True)
 
        ' Gusset #2 insertion parameters (same as for Gusset #1 with the following exceptions)
        '2.  dOffset                = 30 mm
        '19. gussetType             = 1 (flat back)
        '20  bEdgeFillet            = True
        '21. dEdgeFilletRadius      = 1 mm
 
        'Select faces
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0538403893476698, 0.0036701308754914, 0.05530817474488, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0177780871801474, -0.0307393226379986, 0.0341128529187245, True, 0, Nothing, 0)
 
        myFeature1 = Part.FeatureManager.InsertSheetMetalGussetFeature3(True, 0.03, False, swSheetMetalGussetProfileDimType_e.swSheetMetalGussetProfileDimType_IndentDepth, 0.01, 0, False, 0, 0, False, 0.01, 0.003, True, 3 * 0.0175, True, 0.002, True, 0.001, swSheetMetalRibGussetType_e.swSheetMetalRibGussetType_Flat, True, 0.001, TrueTrueTrue)
        Part.ClearSelection2(True)
 
        ' Gusset #3 insertion parameters (same as for Gusset #1 with the following exceptions)
        '2.  dOffset                = 30 mm
        '4.  profDimType            = 1 (length + height dimensioning scheme)
        '5.  dIndentDepth           = 0 mm
        '6.  dLength                = 25 mm
        '7.  bUseAngle              = False
        '8.  dHeight                = 15 mm
        '9   dAngle                 = 0
        '10. bFlipSides             = False
        '19. gussetType             = 1 (flat back)
        '20  bEdgeFillet            = True
        '21. dEdgeFilletRadius      = 1 mm
 
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0538403893476698, 0.0036701308754914, 0.05530817474488, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0177780871801474, -0.0307393226379986, 0.0341128529187245, True, 0, Nothing, 0)
 
        myFeature2 = Part.FeatureManager.InsertSheetMetalGussetFeature3(True, 0.03, False, swSheetMetalGussetProfileDimType_e.swSheetMetalGussetProfileDimType_ProfileDimensions, 0, 0.025, False, 0.015, 0, False, 0.02, 0.003, True, 3 * 0.0175, True, 0.002, True, 0.001, swSheetMetalRibGussetType_e.swSheetMetalRibGussetType_Flat, True, 0.001, TrueTrueTrue)
        Part.ClearSelection2(True)
 
        ' Gusset #4 insertion parameters (same as for Gusset #1 with the following exceptions)
        '2.  dOffset                = 30 mm
        '20  bEdgeFillet            = True
        '21. dEdgeFilletRadius      = 1 mm
 
        'Select orientation and position references
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0538403893476129, -0.00224553153327633, 0.087801420904043, True, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0235965800548001, -0.0307393226379986, 0.0897844682415894, True, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("Line1@Sketch6""EXTSKETCHSEGMENT", -0.00609049483400968, -0.0895139047397037, 0, True, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("Point1@Sketch7""EXTSKETCHPOINT", 0.0180407947995604, -0.0762728416981986, 0, True, 0, Nothing, 0)
 
        myFeature3 = Part.FeatureManager.InsertSheetMetalGussetFeature3(True, 0.03, False, swSheetMetalGussetProfileDimType_e.swSheetMetalGussetProfileDimType_IndentDepth, 0.01, 0, False, 0, 0, False, 0.01, 0.003, True, 3 * 0.0175, True, 0.002, True, 0.001, swSheetMetalRibGussetType_e.swSheetMetalRibGussetType_Rounded, True, 0.001, TrueTrueTrue)
        Part.ClearSelection2(True)
 
        Stop
 
        'Five modifications to gusset feature data:
 
        'a. Modify type, draft, and outer corner fillet options for gusset #1
        boolstatus = Part.Extension.SelectByID2("Sheet Metal Gusset1""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)
 
        swFeatData = swFeat.GetDefinition
        swFeatData.AccessSelections(Part, Nothing)
 
        swFeatData.GussetType = 1 'flat back
        swFeatData.DraftSideFaces = False
        swFeatData.FilletOuterCorners = False 'no outer corner fillet
        Debug.Print("Sheet Metal Gusset1 Flatten Settings")
        Debug.Print("  Override document property settings? " & swFeatData.OverrideDocSettings)
        Debug.Print("  Show center marks? " & swFeatData.ShowCenter)
        Debug.Print("  Show profile? " & swFeatData.ShowProfile)
 
        swFeat.ModifyDefinition(swFeatData, Part, Nothing)
        swFeatData.ReleaseSelectionAccess()
 
        Stop
 
        'b. Modify orientation reference of gusset #3
        boolstatus = Part.Extension.SelectByID2("Sheet Metal Gusset3""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)
 
        swFeatData = swFeat.GetDefinition
        swFeatData.AccessSelections(Part, Nothing)
 
        boolstatus = Part.Extension.SelectByID2("Line1@Sketch6""EXTSKETCHSEGMENT", -0.00609049483400968, -0.0895139047397037, 0, True, 0, Nothing, 0)
 
        Dim refLine As Object
        refLine = Part.SelectionManager.GetSelectedObject6(1, -1)
        swFeatData.ReferenceLine = refLine
 
        swFeat.ModifyDefinition(swFeatData, Part, Nothing)
 
        Stop
 
        'c. Modify legs of gusset #2: select one bend face instead of two flat faces
        boolstatus = Part.Extension.SelectByID2("Sheet Metal Gusset2""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)
 
        swFeatData = swFeat.GetDefinition
        swFeatData.AccessSelections(Part, Nothing)
 
        boolstatus = Part.Extension.SelectByID2("""FACE", 0.03831148650454, -0.0327672470662037, 0.147978181958194, False, 0, Nothing, 0)
 
        Dim newBendFace As Object
        Dim bendfaces(0) As Face2
        bendfaces(0) = Part.SelectionManager.GetSelectedObject6(1, -1)
 
        newBendFace = bendfaces
        swFeatData.SupportingFaces = newBendFace
        Debug.Print("Sheet Metal Gusset2 Flatten Settings")
        Debug.Print("  Override document property settings? " & swFeatData.OverrideDocSettings)
        Debug.Print("  Show center marks? " & swFeatData.ShowCenter)
        Debug.Print("  Show profile? " & swFeatData.ShowProfile)
 
        swFeat.ModifyDefinition(swFeatData, Part, Nothing)
 
        Stop
 
        'd. Modify reference position of gusset #3 - 3 mm away from vertex of hexagonal cut
        boolstatus = Part.Extension.SelectByID2("Sheet Metal Gusset3""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)
 
        swFeatData = swFeat.GetDefinition
        swFeatData.AccessSelections(Part, Nothing)
 
        boolstatus = Part.Extension.SelectByID2("""VERTEX", -0.0538403893475499, -0.0100654290631334, 0.205954465964501, False, 0, Nothing, 0)
 
        Dim refPoint As Object
        refPoint = Part.SelectionManager.GetSelectedObject6(1, -1)
        swFeatData.ReferencePoint = refPoint
        Debug.Print("Sheet Metal Gusset3 Flatten Settings")
        Debug.Print("  Override document property settings? " & swFeatData.OverrideDocSettings)
        Debug.Print("  Show center marks? " & swFeatData.ShowCenter)
        Debug.Print("  Show profile? " & swFeatData.ShowProfile)
 
        swFeat.ModifyDefinition(swFeatData, Part, Nothing)
 
        Stop
 
        'e. Modify type and inner corner fillet options for gusset #4
        boolstatus = Part.Extension.SelectByID2("Sheet Metal Gusset4""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)
 
        swFeatData = swFeat.GetDefinition
        swFeatData.AccessSelections(Part, Nothing)
 
        swFeatData.GussetType = 0 'rounded back
        swFeatData.FilletInnerCorners = False 'no inner corner fillet
        Debug.Print("Sheet Metal Gusset4 Flatten Settings")
        Debug.Print("  Override document property settings? " & swFeatData.OverrideDocSettings)
        Debug.Print("  Show center marks? " & swFeatData.ShowCenter)
        Debug.Print("  Show profile? " & swFeatData.ShowProfile)
 
        swFeat.ModifyDefinition(swFeatData, Part, Nothing)
        swFeatData.ReleaseSelectionAccess()
 
 
    End Sub
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
 
 
End Class

 

 



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