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Set Body for View Example (VBA)

This example shows how to show just one body of a multibody part in a drawing view.

'------------------------------------------------------------------
' Preconditions:
' 1. Open public_documents\tutorial\multibody\multi_inter.sldprt.
' 2. Save the part document as a drawing document:
'    a. Click File > Make Drawing from Part.
'    b. Click OK on the Sheet Format/Size dialog.
'    c. Drag the *Isometric view from the View Palette onto
'       the drawing sheet.
' 3. Select the drawing view.
' 4. Open the Immediate window.
'
' Postconditions:
' 1. Shows one body of the multibody part
'    in the drawing view.
' 2. Examine the drawing and the Immediate window.
'
' NOTE: Because the part document is used elsewhere, do not save
' changes.
'------------------------------------------------------------------

Option Explicit

 

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swSelMgr As SldWorks.SelectionMgr

Dim swView As SldWorks.View

Dim nbrBodies As Long

Dim arrBody As Variant

Dim swBody As SldWorks.Body2

Dim swFace As SldWorks.Face2

Dim swEnt As SldWorks.Entity

Dim swSelData As SldWorks.SelectData

Dim bool As Boolean

Dim arrBodiesIn As Variant

Dim Bodies(0) As Object

Dim i As Long

Dim objType As Long

 

Sub main()

 

Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swSelMgr = swModel.SelectionManager

Set swView = swSelMgr.GetSelectedObject6(1, -1)

If (swView Is Nothing) Then

    MsgBox "View not selected."

    Exit Sub

End If

nbrBodies = swView.GetBodiesCount

    Debug.Print "Number of bodies: " & nbrBodies

    If (nbrBodies < 1) Then

        MsgBox "No bodies in selected view."

        Exit Sub

    End If

arrBody = swView.Bodies

For i = 0 To UBound(arrBody)

    Set swBody = arrBody(i)

    Set swSelData = swSelMgr.CreateSelectData

    swSelData.View = swView

    bool = swBody.Select2(False, swSelData)

        ' Object type 76 is a solid body

        objType = swSelMgr.GetSelectedObjectType3(1, -1)

        If (objType = 76) Then

            Debug.Print " Object type: solid body"

        End If

        If (Not (swSelSOLIDBODIES = swSelMgr.GetSelectedObjectType3(1, -1))) Then

            MsgBox "Solid body not found."

        End If

        Set swFace = swBody.GetFirstFace

        Do While Not swFace Is Nothing

            Set swEnt = swFace

            ' Select using IEntity

            bool = swEnt.Select4(True, swSelData): Debug.Assert bool

            Set swFace = swFace.GetNextFace

        Loop

        Debug.Print "   Name of body: " & swBody.GetSelectionId

    Next i

    

swModel.ClearSelection2 True

 

' Get the bodies from referenced model

Set swModel = swView.ReferencedDocument

arrBody = swModel.GetBodies2(swSolidBody, True)

If (nbrBodies = 1) Then

   swView.Bodies = (arrBody)

Else

   ' Set the body to view

   Set Bodies(0) = arrBody(0)

   arrBodiesIn = Bodies

   swView.Bodies = (arrBodiesIn)

End If

 

swModel.ClearSelection2 True

    

End Sub



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