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Add Along Y Dimension to 3D Sketch Example (VBA)

This example shows how to add a display dimension along the y 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 63.238 mm appears on the y axis starting at

'      (-0.1, 0, 0.01111142101618) while the sketch is in edit mode.

'----------------------------------------------------------------------------

Option Explicit

 

Dim swApp As SldWorks.SldWorks

Dim Part As SldWorks.ModelDoc2

Dim myDisplayDim As SldWorks.DisplayDimension

Dim boolstatus As Boolean

Dim longstatus As Long

Sub main()

Set swApp = Application.SldWorks

boolstatus = swApp.ResetUntitledCount(0, 0, 0)

Set 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

Set Part = swApp.ActiveDoc

Part.SketchManager.Insert3DSketch True

Dim vSkLines As Variant

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 Variant

Dim points() As Double

ReDim points(0 To 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 SldWorks.SketchSegment

Set 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)

Set myDisplayDim = Part.SketchManager.AddAlongYDimension(-0.1, 0, 0.01111142101618)

Part.ClearSelection2 True

Part.ViewZoomtofit2

End Sub



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