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Set Profile for Structural Member Example (VBA)

This example shows how to set the profile for a structural member.

' Preconditions:
' 1. Open public_documents\tutorial\api\weldment_box3.sldprt.
' 2. Verify that the path specified for the weldment profile
'    exists.
' 3. Right-click Structural Member1, select Edit Feature,
'    examine Selections, and click OK.
' Postconditions:
' 1. Changes the weldment profile to the specified weldment
'    profile.
' 2. To verify step 1, right-click StructuralMember1, select
'    Edit Feature, examine Selections, and click OK.
' NOTE: Because the part is used elsewhere, do  not save
' changes.
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSelMgr As SldWorks.SelectionMgr
Dim swWeldFeat As SldWorks.Feature
Dim swWeldFeatData As SldWorks.StructuralMemberFeatureData
Dim boolstatus As Boolean
Sub main()
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swSelMgr = swModel.SelectionManager
    Set swModelDocExt = swModel.Extension
    boolstatus = swModelDocExt.SelectByID2("Structural Member1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
    Set swWeldFeat = swSelMgr.GetSelectedObject6(1, 0)
    Set swWeldFeatData = swWeldFeat.GetDefinition
    swWeldFeatData.AccessSelections swModel, Nothing
    swWeldFeatData.WeldmentProfilePath = "C:\Program Files\SolidWorks Corp\SolidWorks\lang\english\weldment profiles\iso\pipe\26.9 x 3.2.sldlfp"
    boolstatus = swWeldFeat.ModifyDefinition(swWeldFeatData, swModel, Nothing)
End Sub

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