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Insert Sheet Metal Gusset Feature Example (VBA)

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.
' ---------------------------------------------------------------------------

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim myFeature As SldWorks.Feature
Dim myFeature1 As SldWorks.Feature
Dim myFeature2 As SldWorks.Feature
Dim myFeature3 As SldWorks.Feature
Dim myFeature4 As SldWorks.Feature
Dim swFeat As SldWorks.Feature
Dim swFeatData As SldWorks.SMGussetFeatureData
Dim boolstatus As Boolean
Option Explicit

Sub main()

    Set swApp = Application.SldWorks
    Set Part = swApp.ActiveDoc
   

    boolstatus = Part.Extension.SelectByID2("", "FACE", -5.38403893476698E-02, 3.6701308754914E-03, 0.05530817474488, False, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("", "FACE", -1.77780871801474E-02, -3.07393226379986E-02, 3.41128529187245E-02, 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
   

    Set myFeature = Part.FeatureManager.InsertSheetMetalGussetFeature3(True, 0.05, False, swSheetMetalGussetProfileDimType_IndentDepth, 0.01, 0, False, 0, 0, True, 0.01, 0.003, True, 3 * 0.0175, True, 0.002, True, 0.001, swSheetMetalRibGussetType_Rounded, False, 0, True, True, True)
    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", -5.38403893476698E-02, 3.6701308754914E-03, 0.05530817474488, False, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("", "FACE", -1.77780871801474E-02, -3.07393226379986E-02, 3.41128529187245E-02, True, 0, Nothing, 0)
   

    Set myFeature1 = Part.FeatureManager.InsertSheetMetalGussetFeature3(True, 0.03, False, swSheetMetalGussetProfileDimType_IndentDepth, 0.01, 0, False, 0, 0, False, 0.01, 0.003, True, 3 * 0.0175, True, 0.002, True, 0.001, swSheetMetalRibGussetType_Flat, True, 0.001, True, True, True)
    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", -5.38403893476698E-02, 3.6701308754914E-03, 0.05530817474488, False, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("", "FACE", -1.77780871801474E-02, -3.07393226379986E-02, 3.41128529187245E-02, True, 0, Nothing, 0)
   

    Set myFeature2 = Part.FeatureManager.InsertSheetMetalGussetFeature3(True, 0.03, False, 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_Flat, True, 0.001, True, True, True)
    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", -5.38403893476129E-02, -2.24553153327633E-03, 0.087801420904043, True, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("", "FACE", -2.35965800548001E-02, -3.07393226379986E-02, 8.97844682415894E-02, True, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Line1@Sketch6", "EXTSKETCHSEGMENT", -6.09049483400968E-03, -8.95139047397037E-02, 0, True, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Point1@Sketch7", "EXTSKETCHPOINT", 1.80407947995604E-02, -7.62728416981986E-02, 0, True, 0, Nothing, 0)

    Set myFeature3 = Part.FeatureManager.InsertSheetMetalGussetFeature3(True, 0.03, False, swSheetMetalGussetProfileDimType_IndentDepth, 0.01, 0, False, 0, 0, False, 0.01, 0.003, True, 3 * 0.0175, True, 0.002, True, 0.001, swSheetMetalRibGussetType_Rounded, True, 0.001, True, True, True)
    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)
        Set swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)
       

        Set 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)
        Set swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)
       

        Set swFeatData = swFeat.GetDefinition
        swFeatData.AccessSelections Part, Nothing

        boolstatus = Part.Extension.SelectByID2("Line1@Sketch6", "EXTSKETCHSEGMENT", -6.09049483400968E-03, -8.95139047397037E-02, 0, True, 0, Nothing, 0)

        Dim refLine As Variant
        Set 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)
        Set swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)

        Set swFeatData = swFeat.GetDefinition
        swFeatData.AccessSelections Part, Nothing
       

        boolstatus = Part.Extension.SelectByID2("", "FACE", 0.03831148650454, -3.27672470662037E-02, 0.147978181958194, False, 0, Nothing, 0)

        Dim newBendFace As Variant
        Dim bendfaces(0 To 1) As Object
        Dim jj As Integer
        For jj = 0 To 1
           Set bendfaces(jj) = Part.SelectionManager.GetSelectedObject6(jj + 1, -1)
        Next jj
        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)
        Set swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)
       

        Set swFeatData = swFeat.GetDefinition
        swFeatData.AccessSelections Part, Nothing

        boolstatus = Part.Extension.SelectByID2("", "VERTEX", -5.38403893475499E-02, -1.00654290631334E-02, 0.205954465964501, False, 0, Nothing, 0)
   

        Dim refPoint As Variant
        Set 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)
        Set swFeat = Part.SelectionManager.GetSelectedObject6(1, -1)

        Set 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



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