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Show Dimensions in Drawing Sheet Example (VBA)

This example shows how to show all of the dimensions in a drawing sheet whether or not the dimensions are hidden or shown.

 

'----------------------------------------------------------

'

' Problem:

'       In the SolidWorks user interface, you can hide a dimension in a

'       drawing view through the shortcut menu.  The corresponding

'       API to do this is IModelDoc2::HideDimension.

'

'       However, in the use interface, there is no ready to show

'       a hidden dimension because it must be selected.

'

'       This example shows how to traverse all display dimensions

'       on a drawing sheet and show them.

'

' Preconditions: Drawing is open and dimensions are marked for drawing.

'

' Postconditions: None

'

' NOTE: Dimension is not shown if it is on a layer that

'       is hidden.

'

'----------------------------------------------------------

Option Explicit

Public Enum swAnnotationVisibilityState_e

    swAnnotationVisibilityUnknown = 0

    swAnnotationVisible = 1

    swAnnotationHalfHidden = 2

    swAnnotationHidden = 3

End Enum

Public Enum swAnnotationType_e

    swCThread = 1

    swDatumTag = 2

    swDatumTargetSym = 3

    swDisplayDimension = 4

    swGTol = 5

    swNote = 6

    swSFSymbol = 7

    swWeldSymbol = 8

    swCustomSymbol = 9

    swDowelSym = 10

    swLeader = 11

    swBlock = 12

    swCenterMarkSym = 13

    swTableAnnotation = 14

    swCenterLine = 15

    swDatumOrigin = 16

End Enum

Sub ProcessDrawing _

( _

    swApp As SldWorks.SldWorks, _

    swModel As SldWorks.ModelDoc2, _

    swView As SldWorks.View _

)

    Dim swAnn As SldWorks.Annotation

    

    Debug.Print "  " & swView.Name

    

    Set swAnn = swView.GetFirstAnnotation2

    Do While Not Nothing Is swAnn

        If swDisplayDimension = swAnn.GetType Then

            Debug.Print "    " & swAnn.GetName

            

            swAnn.Visible = swAnnotationVisible

        End If

        

        Set swAnn = swAnn.GetNext2

    Loop

End Sub

Sub main()

    Dim swApp                       As SldWorks.SldWorks

    Dim swModel                     As SldWorks.ModelDoc2

    Dim swDraw                      As SldWorks.DrawingDoc

    Dim swView                      As SldWorks.View

    Dim bRet                        As Boolean

    

    Set swApp = Application.SldWorks

    Set swModel = swApp.ActiveDoc

    Set swDraw = swModel

            

    Debug.Print "File = " & swModel.GetPathName

    

    Set swView = swDraw.GetFirstView

    Do While Not Nothing Is swView

        

        ProcessDrawing swApp, swDraw, swView

        

        Set swView = swView.GetNextView

    Loop

    

    swModel.GraphicsRedraw2

End Sub

'-----------------------------------------------



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