Add Along X Dimension to 3D Sketch Example (VB.NET)
This example shows how to add a display dimension along the x axis in
a 3D sketch.
'----------------------------------------------------------------------------
' Preconditions:
' 1.
Open SolidWorks.
' 2.
Verify the location of the part template.
' Postconditions:
' 1.
Click the green check mark in the Modify dimension dialog
' (look for the
hidden dialog behind your other windows).
' 2.
3DSketch1 is in edit mode and contains a spline and a corner rectangle.
' 3.
The display dimension of 84.455mm appears along the x axis starting at
'
(0.05, -0.091, 0.001)
while the sketch is in edit mode.
'---------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System
Partial Class SolidWorksMacro
Dim
Part As ModelDoc2
Dim
myDisplayDim As DisplayDimension
Dim
myDimension As Object
Dim
boolstatus As Boolean
Dim
longstatus As Integer
Sub
main()
boolstatus
= swApp.ResetUntitledCount(0, 0, 0)
Part
= swApp.NewDocument("C:\Documents and Settings\All Users\Application
Data\SolidWorks\SolidWorks 2010\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.AddAlongXDimension(0.05,
-0.091, 0.001)
Part.ClearSelection2(True)
Part.ViewZoomtofit2()
End
Sub
Public
swApp As SldWorks
End Class