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Get Custom Property Values on Weldment Cut-list Folders Example (VBA)

This example shows how to get all of the custom property values on the weldment cut-list folders of a part in an assembly.



' Preconditions:

' 1. Assembly is open.

' 2. At least one part in the assembly

'    has a weldment cut-list folder

'    that has custom properties.


' Postconditions: None


Option Explicit


Dim swApp As SldWorks.SldWorks

Dim Part As SldWorks.ModelDoc2

Dim SelMgr As SldWorks.SelectionMgr

Dim boolstatus As Boolean

Dim longstatus As Long, longwarnings As Long


Sub VisitFeatureCustomProperties(docFeat As SldWorks.Feature)

    Dim custPropMgr As SldWorks.CustomPropertyManager

    Dim propNames As Variant

    Dim vName As Variant

    Dim propName As String

    Dim Value As String

    Dim resolvedValue As String


    Set custPropMgr = docFeat.CustomPropertyManager

    If Not custPropMgr Is Nothing Then

        propNames = custPropMgr.GetNames

        If Not IsEmpty(propNames) Then

            Debug.Print docFeat.Name, docFeat.GetTypeName

            For Each vName In propNames

                propName = vName

                Call custPropMgr.Get2(propName, Value, resolvedValue)

                Debug.Print "", "", propName, Value, resolvedValue

            Next vName

        End If

    End If

End Sub


Sub VisitDocWeldmentProperties(compDoc As SldWorks.ModelDoc2)

    Dim thisFeat As SldWorks.Feature

    Dim thisSubFeat As SldWorks.Feature

    Dim cutFolder As SldWorks.BodyFolder


    Set thisFeat = compDoc.FirstFeature

    Do While Not thisFeat Is Nothing


        Set thisSubFeat = thisFeat.GetFirstSubFeature

        Do While Not thisSubFeat Is Nothing


            If thisSubFeat.GetTypeName = "CutListFolder" Then

                Set cutFolder = thisSubFeat.GetSpecificFeature2

            End If

            If Not cutFolder Is Nothing Then

                If cutFolder.GetBodyCount > 0 Then

                    Call VisitFeatureCustomProperties(thisSubFeat)

                End If

            End If


            Set thisSubFeat = thisSubFeat.GetNextSubFeature


        Set thisFeat = thisFeat.GetNextFeature


End Sub


Sub main()

Set swApp = Application.SldWorks


    Set Part = swApp.ActiveDoc

    Set SelMgr = Part.SelectionManager

    boolstatus = Part.Extension.SelectByID2("1-1@Assemblage", "COMPONENT", 0, 0, 0, False, 0, Nothing, 0)


    Dim selComp As SldWorks.Component2

    Dim refConfig As String

    Dim compDoc As SldWorks.ModelDoc2


    Set selComp = SelMgr.GetSelectedObject6(1, -1)

    Set compDoc = selComp.GetModelDoc


    Dim configNames As Variant

    Dim vName As Variant

    Dim configName As String

    configNames = compDoc.GetConfigurationNames()

    For Each vName In configNames

        configName = vName

        Debug.Print "-----------------------------------------------"

        Debug.Print "Configuration: " + configName

        boolstatus = compDoc.ShowConfiguration2(configName)

        Call VisitDocWeldmentProperties(compDoc)

    Next vName


End Sub

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