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Select Entity in Drawing View Example (VBA)

This example shows how to select any of these entities in a drawing view: model face, edge, or vertex.




' Problem:

'       Selection of a model geometry in the context of a drawing

'       view can be quite problematic. To address this, use   

'       IView::SelectEntity


'       Thus, given an entity in the context of the model, this

'       method selects the entity in the context of the drawing

'       view.


'       This code shows how to use this method to assist in

'       adding a dimension to a drawing view.


' Preconditions:

'       (1) Part or assembly is open.

'       (2) Assembly is fully resolved.

'       (3) Face, edge or vertex is selected.


' Postconditions:

'       (1) New drawing is created with three views.

'       (2) If possible, the previously selected face, edge or vertex

'           is dimensioned in the first drawing view.


' NOTE:  The dimension is not guaranteed to be created if, for

'        example, a face is selected.



Option Explicit


Public Enum swDwgTemplates_e

    swDwgTemplateAsize = 0

    swDwgTemplateAsizeVertical = 1

    swDwgTemplateBsize = 2

    swDwgTemplateCsize = 3

    swDwgTemplateDsize = 4

    swDwgTemplateEsize = 5

    swDwgTemplateA4size = 6

    swDwgTemplateA4sizeVertical = 7

    swDwgTemplateA3size = 8

    swDwgTemplateA2size = 9

    swDwgTemplateA1size = 10

    swDwgTemplateA0size = 11

    swDwgTemplateCustom = 12

    swDwgTemplateNone = 13

End Enum

Public Enum swDwgPaperSizes_e

    swDwgPaperAsize = 0

    swDwgPaperAsizeVertical = 1

    swDwgPaperBsize = 2

    swDwgPaperCsize = 3

    swDwgPaperDsize = 4

    swDwgPaperEsize = 5

    swDwgPaperA4size = 6

    swDwgPaperA4sizeVertical = 7

    swDwgPaperA3size = 8

    swDwgPaperA2size = 9

    swDwgPaperA1size = 10

    swDwgPaperA0size = 11

    swDwgPapersUserDefined = 12

End Enum


Sub main()


    Const sPathToTemplate       As String = "C:\Program Files\SolidWorks\data\templates\drawing.drwdot"


    Const nYoffset              As Double = 0.01


    Dim swApp                   As SldWorks.SldWorks

    Dim swModel                 As SldWorks.ModelDoc2

    Dim swSelMgr                As SldWorks.SelectionMgr

    Dim swEnt                   As SldWorks.entity


    Dim swDraw                  As SldWorks.DrawingDoc

    Dim swDrawModel             As SldWorks.ModelDoc2

    Dim swView                  As SldWorks.view

    Dim vOutline                 As Variant

    Dim swDispDim               As SldWorks.DisplayDimension


    Dim nXpos                   As Double

    Dim nYpos                   As Double


    Dim bRet                    As Boolean


    Set swApp = CreateObject("SldWorks.Application")

    Set swModel = swApp.ActiveDoc

    Set swSelMgr = swModel.SelectionManager

    Set swEnt = swSelMgr.GetSelectedObject5(1)


    Set swDraw = swApp.NewDrawing2(swDwgTemplateCustom, sPathToTemplate, swDwgPaperA1size, 0#, 0#)

    Set swDrawModel = swDraw


    bRet = swDraw.Create3rdAngleViews2(swModel.GetPathName)

    Debug.Assert bRet


    Set swView = swDraw.GetFirstView

    Set swView = swView.GetNextView


    bRet = swView.SelectEntity(swEnt, False)

    Debug.Assert bRet


    ' Work out where to place dimension -

    ' midway across view and slightly above

    vOutline = swView.GetOutline

    nXpos = (vOutline(0) + vOutline(2)) / 2#

    nYpos = vOutline(3) + nYoffset


    ' This depends on the orientation of the entity in the drawing view.

    ' Thus, could be NULL.


    ' Will also create the dimension even if the entity is not

    ' visible in the drawing view

    Set swDispDim = swDrawModel.AddDimension2(nXpos, nYpos, 0#)

End Sub


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