Add Along Z Dimension to 3D Sketch Example (VB.NET)
This example shows how to add a display dimension along the z 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 64.809 mm appears on the z axis starting at
' (-0.03841894197919,
-0.03273212874668, 0.042510877252)
' 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
boolstatus As Boolean
Dim
longstatus As Long
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.AddAlongZDimension(-0.03841894197919,
-0.03273212874668, 0.042510877252)
Part.ClearSelection2(True)
Part.ViewZoomtofit2()
End
Sub
Public
swApp As SldWorks
End Class