Modify Break Corner Feature Example (VB.NET)
This example shows how to create and modify a break corner feature in a sheet metal
part.
'---------------------------------------------------
' Preconditions:
' 1. Verify that the specified part document exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens the specified document.
' 2. Selects a face on Edge-Flange1.
' 3. Creates a break corner feature.
' 4. Unsuppresses the flat pattern feature.
' 5. Accesses the break corner feature and
' and modifies it.
' 6. Suppresses the flat pattern feature.
' 7. Examine the graphics area and the Immediate window.
'
' NOTE: Because the part document is used elsewhere,
' do not save any changes.
'----------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
Partial Class SolidWorksMacro
Public Sub Main()
Dim swModel As ModelDoc2
Dim swModelDocExt As ModelDocExtension
Dim swSelectionMgr As SelectionMgr
Dim swFeature As Feature
Dim swBreakCornerFeatureData As BreakCornerFeatureData
Dim fileName As String
Dim status As Boolean
Dim errors As Integer
Dim warnings As Integer
fileName = "C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\api\sm1-remove-edges.sldprt"
swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
swModelDocExt = swModel.Extension
status = swModelDocExt.SelectByID2("", "FACE", -0.111589911985732, 0.0979999999999563, 0.0841212722518208, True, 0, Nothing, 0)
swModel.InsertSheetMetalBreakCorner(swBreakCornerTypes_e.swBreakCornerTypeChamfer, 0.005)
'Select and unsuppress the flat pattern feature
status = swModelDocExt.SelectByID2("Flat-Pattern1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
swModel.EditUnsuppress2()
swModel.ClearSelection2(True)
'Select the break corner feature
'and change some of its properties
status = swModelDocExt.SelectByID2("Break-Corner1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
swSelectionMgr = swModel.SelectionManager
swFeature = swSelectionMgr.GetSelectedObject6(1, 0)
swBreakCornerFeatureData = swFeature.GetDefinition
status = swBreakCornerFeatureData.AccessSelections(swModel, Nothing)
Debug.Print("AccessSelections: " & status)
Debug.Print("")
Debug.Print(" -------------Original--------------")
Debug.Print(" CenteredOnBendLines: " & swBreakCornerFeatureData.CenteredOnBendLines)
Debug.Print(" InternalCornersOnly: " & swBreakCornerFeatureData.InternalCornersOnly)
swBreakCornerFeatureData.InternalCornersOnly = True
swBreakCornerFeatureData.CenteredOnBendLines = True
Debug.Print("")
Debug.Print(" -------------Modified--------------")
Debug.Print(" CenteredOnBendLines: " & swBreakCornerFeatureData.CenteredOnBendLines)
Debug.Print(" InternalCornersOnly: " & swBreakCornerFeatureData.InternalCornersOnly)
status = swFeature.ModifyDefinition(swBreakCornerFeatureData, swModel, Nothing)
Debug.Print("")
Debug.Print("ModifyDefinition: " & status)
swModel.ClearSelection2(True)
'Select and suppress the flat pattern feature
status = swModelDocExt.SelectByID2("Flat-Pattern1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
swModel.EditSuppress2()
swModel.ClearSelection2(True)
End Sub
''' <summary>
''' The SldWorks swApp variable is pre-assigned for you.
''' </summary>
Public swApp As SldWorks
End Class