Hide Table of Contents

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



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Get Corner Points of a Reference Plane Example (VBA)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2012 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.