This example shows how to insert a sheet metal gusset feature and modify its data.
'----------------------------------------------------------------------------
' Preconditions:
' 1. Open public_documents\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, 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", -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, 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", -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, 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", -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, 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)
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