Add Along Y Dimension to 3D Sketch Example (VB.NET)
This example shows how to add a display dimension along the y axis in
a 3D sketch.
'----------------------------------------------------------------------------
' Preconditions: Verify that the specified part template exists.
'
' Postconditions:
' 1. Opens a new part document.
' 2. Creates a 3D sketch.
' 3. Click the green check mark in the Modify dimension dialog
' (If you don't see the dialog, look for it behind other open windows).
' 4. Puts 3DSketch1 in edit mode; 3DSketch1 contains a spline and a
' corner rectangle.
' 5. Displays the display dimension of 63.24 mm on the y axis starting at
' (-0.1, 0, 0.01111142101618) while the sketch is in edit mode.
' 6. Examine the graphics area.
'----------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Partial Class SolidWorksMacro
Public Sub main()
Dim Part As ModelDoc2
Dim myDisplayDim As DisplayDimension
Dim boolstatus As Boolean
Dim longstatus As Integer
longstatus = swApp.ResetUntitledCount(0, 0, 0)
Part = swApp.NewDocument("C:\Documents and Settings\All Users\Application Data\SOLIDWORKS\SOLIDWORKS 2015\templates\Part.prtdot", 0, 0, 0)
swApp.ActivateDoc2("Part1", False, longstatus)
Part = swApp.ActiveDoc
Part.SketchManager.Insert3DSketch(True)
Dim vSkLines As Object
vSkLines = Part.SketchManager.CreateCornerRectangle(-0.05171778666374, 0.01933785938058, 0.03, 0.08445537697179, -0.04142795937025, -0.03)
boolstatus = Part.Extension.SelectByID2("Right Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
Part.ClearSelection2(True)
Dim pointArray As Object
Dim points(11) As Double
points(0) = 0
points(1) = -0.03591009660795
points(2) = 0.04608246573503
points(3) = 0
points(4) = 0.0147420284178
points(5) = 0.005170989573514
points(6) = 0
points(7) = -0.006478053228363
points(8) = -0.04282131900055
points(9) = 0
points(10) = -0.02294509596464
points(11) = -0.09396066420243
pointArray = points
Dim skSegment As SketchSegment
skSegment = Part.SketchManager.CreateSpline2((pointArray), True)
Part.SketchManager.InsertSketch(True)
boolstatus = Part.Extension.SelectByID2("3DSketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)
Part.EditSketch()
boolstatus = Part.Extension.SelectByID2("Point5", "SKETCHPOINT", 0, -0.03591009660795, 0.04608246573503, False, 0, Nothing, 0)
boolstatus = Part.Extension.SelectByID2("Point4", "SKETCHPOINT", 0.08445537697179, 0.02732744880518, -0.01872625210654, True, 0, Nothing, 0)
myDisplayDim = Part.SketchManager.AddAlongYDimension(-0.1, 0, 0.01111142101618)
Part.ClearSelection2(True)
Part.ViewZoomtofit2()
End Sub
''' <summary>
''' The SldWorks swApp variable is pre-assigned for you.
''' </summary>
Public swApp As SldWorks
End Class