Get and Set Whether to Hide Cutting Line Shoulders Example (VB.NET)
This example shows how to get and set whether to hide cutting line shoulders
in a section view.
'--------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the part and templates exist.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens the part.
' 2. Creates a drawing of the part.
' 3. Creates a section view.
' 4. Gets and sets whether to hide cutting line shoulders in the section
' view.
' 5. Examine the Immediate window.
'
' NOTE: Because the part is used elsewhere, do not save it or the drawing.
'--------------------------------------------------------------------------
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 swDrawing As DrawingDoc
Dim swSheet As Sheet
Dim swView As View
Dim swModelDocExt As ModelDocExtension
Dim swSketchSegment As SketchSegment
Dim swSketchMgr As SketchManager
Dim swSectionView As DrSection
Dim status As Boolean
Dim errors As Integer
Dim warnings As Integer
Dim fileName As String
Dim swSheetWidth As Double
Dim swSheetHeight As Double
Dim drawingTemplate As String
Dim sheetTemplate As String
'Open part
fileName = "C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\api\cam roller.sldprt"
swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
'Create drawing of part
swSheetWidth = 1.189
swSheetHeight = 0.841
drawingTemplate = "C:\ProgramData\SolidWorks\SOLIDWORKS 2017\templates\Drawing.drwdot"
swDrawing = swApp.NewDocument(drawingTemplate, swDwgPaperSizes_e.swDwgPapersUserDefined, swSheetWidth, swSheetHeight)
swSheet = swDrawing.GetCurrentSheet()
swSheet.SetProperties2(swDwgPaperSizes_e.swDwgPapersUserDefined, swDwgTemplates_e.swDwgTemplateCustom, 1, 2, False, swSheetWidth, swSheetHeight, True)
sheetTemplate = "C:\ProgramData\SolidWorks\SOLIDWORKS 2017\lang\english\sheetformat\a0 - iso.slddrt"
swSheet.SetTemplateName(sheetTemplate)
swSheet.ReloadTemplate(True)
status = swDrawing.GenerateViewPaletteViews(fileName)
swView = swDrawing.DropDrawingViewFromPalette2("*Left", 0.580930433566434, 0.431525272727273, 0)
'Create section view
swDrawing = swApp.ActiveDoc
status = swDrawing.ActivateView("Drawing View1")
swModel.ClearSelection2(True)
swModel = swDrawing
swSketchMgr = swModel.SketchManager
swSketchSegment = swSketchMgr.CreateLine(0.0#, 0.0#, 0.0#, 0.012168, 0.021283, 0.0#)
swSketchSegment = swSketchMgr.CreateLine(0.0#, 0.0#, 0.0#, 0.024347, -0.010966, 0.0#)
swModelDocExt = swModel.Extension
status = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT", 0.690604633175108, 0.625483883858213, 0, False, 0, Nothing, 0)
status = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0.747211061353527, 0.357889859742052, 0, True, 0, Nothing, 0)
swView = swDrawing.CreateSectionViewAt5(0.676815388637685, 0.116110180826413, 0, "A", swCreateSectionViewAtOptions_e.swCreateSectionView_OffsetSection, Nothing, 0)
status = swDrawing.ActivateView("Drawing View2")
swModel.ClearSelection2(True)
'Get section view and get and set whether to hide cutting line shoulders
swSectionView = swView.GetSection
If swSectionView.CuttingLineShoulders Then
Debug.Print("Hide cutting line shoulders = True")
Debug.Print("Setting hide cutting line shoulders to False")
swSectionView.CuttingLineShoulders = False
Debug.Print(" Hide cutting line shoulders = " & swSectionView.CuttingLineShoulders)
Else
Debug.Print("Hide cutting line shoulders = False")
Debug.Print("Setting hide cutting line shoulders to True")
swSectionView.CuttingLineShoulders = True
Debug.Print(" Hide cutting line shoulders = " & swSectionView.CuttingLineShoulders)
End If
End Sub
''' <summary>
''' The SldWorks swApp variable is pre-assigned for you.
''' </summary>
Public swApp As SldWorks
End Class