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Create Plane thru 3 Points In-context Example (VBA)

This example shows how to create a plane through 3 points in-context.




' Preconditions:

'       (1) Assembly is open.

'       (2) Assembly is fully resolved.

'       (3) Component is selected.


' Postconditions: Plane, passing through three points,

'                 is created in the selected component.



Option Explicit


'  Possible status values for AssemblyDoc::EditPart2

Public Enum swEditPartCommandStatus_e

    swEditPartFailure = -1

    swEditPartAsmMustBeSaved = -2

    swEditPartCompMustBeSelected = -3

    swEditPartCompMustBeResolved = -4

    swEditPartCompMustHaveWriteAccess = -5

    swEditPartSuccessful = 0

    swEditPartCompNotPositioned = &H1

End Enum


Sub main()


    Dim swApp                   As SldWorks.SldWorks

    Dim swModel                 As SldWorks.ModelDoc2

    Dim swAssy                  As SldWorks.AssemblyDoc

    Dim swEditModel             As SldWorks.ModelDoc2

    Dim swSelMgr                As SldWorks.SelectionMgr

    Dim swSelData               As SldWorks.SelectData

    Dim swPart                  As SldWorks.PartDoc

    Dim swSketchPt1             As SldWorks.SketchPoint

    Dim swSketchPt2             As SldWorks.SketchPoint

    Dim swSketchPt3             As SldWorks.SketchPoint

    Dim swPlane                 As SldWorks.refPlane

    Dim nRetVal                 As Long

    Dim nInfo                   As Long

    Dim bRet                    As Boolean


    Set swApp = CreateObject("SldWorks.Application")

    Set swModel = swApp.ActiveDoc

    Set swSelMgr = swModel.SelectionManager

    Set swSelData = swSelMgr.CreateSelectData

    Set swAssy = swModel


    ' start in-context edit

    nRetVal = swAssy.EditPart2(True, False, nInfo)

    Debug.Assert swEditPartSuccessful = nRetVal


    Set swEditModel = swModel


    ' Turn off snapping

    swEditModel.SetAddToDB True


    ' Insert part/component 3D sketch in-context

    swEditModel.Insert3DSketch2 True


    ' Create points in part

    Set swSketchPt1 = swEditModel.CreatePoint2(0#, 0.02123307340457, 0.005485856156458)

    Set swSketchPt2 = swEditModel.CreatePoint2(0.04415646169588, 0.01166034702997, -0.00770979679615)

    Set swSketchPt3 = swEditModel.CreatePoint2(0#, -0.006247647329005, 0.007641244473859)


    ' Exit sketch but in assembly

    ' This gets you to editing part/component in-context

    swModel.Insert3DSketch2 True


    ' Restore snapping

    swEditModel.SetAddToDB False


    swModel.ClearSelection2 True

    bRet = swSketchPt1.Select4(True, swSelData): Debug.Assert bRet

    bRet = swSketchPt2.Select4(True, swSelData): Debug.Assert bRet

    bRet = swSketchPt3.Select4(True, swSelData): Debug.Assert bRet


    ' Create plane in part/component

    Set swPlane = swModel.CreatePlaneThru3Points3(True)

    Debug.Assert Not swPlane Is Nothing


    ' Go back to assembly

    ' End in-context edit


End Sub


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