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Get Corner Points of a Reference Plane Example (VBA)

This example shows how to obtain the 4 corner points of a reference plane.


' Preconditions: The specified file exists.


' Postconditions:

' 1. A 3DSketch1 containing 4 corner points of the reference plane is created.

' 2. The Immediate Window displays the coordinates of each corner point.


' NOTE: Do not save the part as it is used in a SolidWorks tutorial.


Option Explicit

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim boolstatus As Boolean

Dim swFeature As SldWorks.Feature

Dim swRefPlane As SldWorks.RefPlane

Dim swModelExt As SldWorks.ModelDocExtension

Dim swSelMgr As SldWorks.SelectionMgr

Dim vMathPoints As Variant

Dim vArrayData As Variant

Dim pMathPoint As SldWorks.MathPoint

Dim i As Integer

Dim swSketch As SldWorks.Sketch

Dim sketchMgr As SldWorks.SketchManager

Dim sketchPt As SldWorks.SketchPoint

Dim swRefPlaneFeatData As SldWorks.RefPlaneFeatureData

Dim filename As String

Dim errors As swFileLoadError_e

Dim warnings As swFileLoadWarning_e


Sub main()

    filename = "C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\swutilities\bracket_a.sldprt"

    Set swApp = Application.SldWorks

    Set swModel = swApp.OpenDoc6(filename, swDocPART, swOpenDocOptions_Silent, "", errors, warnings)

    Set swModelExt = swModel.Extension

    Set swSelMgr = swModel.SelectionManager

    Set sketchMgr = swModel.SketchManager

    boolstatus = swModelExt.SelectByID2("Plane4", "PLANE", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)

    Set swFeature = swSelMgr.GetSelectedObject5(1)

    Set swRefPlane = swFeature.GetSpecificFeature2


    vMathPoints = swRefPlane.CornerPoints 'Four (4) MathPoint objects are always returned


    sketchMgr.Insert3DSketch True

    For i = 0 To UBound(vMathPoints)

        vArrayData = vMathPoints(i).ArrayData

        Debug.Print " Point x = " & vArrayData(0)

        Debug.Print " Point y = " & vArrayData(1)

        Debug.Print " Point z = " & vArrayData(2)


        Set sketchPt = sketchMgr.CreatePoint(vArrayData(0), vArrayData(1), vArrayData(2))


    Next i


        sketchMgr.Insert3DSketch True

End Sub

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