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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)


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


End Sub

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