Find Attribute Example (VB.NET)
This example shows how to find an attribute on the selected entity.
'-------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified part document to open exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens the specified part document.
' 2. Selects Cut-Extrude3.
' 3. Adds attribute att 1 to the selected feature.
' 4. Rebuilds the part.
' 5. Finds attribute att 1.
' 6. Examine the Immediate window.
'
' NOTE: Because the part is used elsewhere, do not save changes.
'----------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
Partial Class SolidWorksMacro
Public Sub main()
'1 = invisible
'0 = visible
Const CreateVisible As Integer = 0
Const AttDefName As String = "XML_string"
Const AttLenDimName As String = "att_name"
Const AttLenValueName As String = "att_value"
Const AttRootName As String = "att"
Dim swModel As ModelDoc2
Dim swModelDocExt As ModelDocExtension
Dim swSelMgr As SelectionMgr
Dim swFeat As Feature
Dim swEnt As Entity
Dim swAttDef As AttributeDef
Dim swAtt As SolidWorks.Interop.sldworks.Attribute = Nothing
Dim swParamName As Parameter
Dim swParamValue As Parameter
Dim AttName As String = ""
Dim i As Integer
Dim bRet As Boolean
Dim fileName As String
Dim errors As Integer
Dim warnings As Integer
'Open part document
fileName = "C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\smartcomponents\bearing.sldprt"
swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
'Select feature
swModelDocExt = swModel.Extension
bRet = swModelDocExt.SelectByID2("Cut-Extrude3", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
swSelMgr = swModel.SelectionManager
swFeat = swSelMgr.GetSelectedObject6(1, -1)
swEnt = swFeat
'Set attribute att 1
swAttDef = swApp.DefineAttribute(AttDefName)
bRet = swAttDef.AddParameter(AttLenDimName, swParamType_e.swParamTypeString, 0.0#, 0)
bRet = swAttDef.AddParameter(AttLenValueName, swParamType_e.swParamTypeDouble, 0.0#, 0)
bRet = swAttDef.Register
While swAtt Is Nothing
' Get a unique attribute name
i = i + 1
AttName = AttRootName + Str(i)
swAtt = swAttDef.CreateInstance5(swModel, swEnt, AttName, CreateVisible, swInConfigurationOpts_e.swThisConfiguration)
End While
swParamName = swAtt.GetParameter(AttLenDimName)
swParamValue = swAtt.GetParameter(AttLenValueName)
bRet = swParamName.SetStringValue2(AttName & " - " & AttLenDimName, swInConfigurationOpts_e.swAllConfiguration, "")
bRet = swParamValue.SetDoubleValue2(i * 10, swInConfigurationOpts_e.swAllConfiguration, "")
If Not swAtt Is Nothing Then
Debug.Print("Attribute " & AttName & " created.")
Else
Debug.Print("Attribute " & AttName & " not created.")
End If
swModel.ForceRebuild3(True)
'Find attribute att 1
bRet = swModelDocExt.SelectByID2("att 1", "ATTRIBUTE", 0, 0, 0, False, 0, Nothing, 0)
swFeat = swSelMgr.GetSelectedObject6(1, -1)
'Limit search in case attribute does not exist
While swAtt Is Nothing And i < 300
swAtt = swEnt.FindAttribute(swAttDef, i)
i = i + 1
End While
If Not swAtt Is Nothing Then
If False = swAtt.GetEntityState(swAssociatedEntityStates_e.swIsEntityInvalid) And False = swAtt.GetEntityState(swAssociatedEntityStates_e.swIsEntitySuppressed) And False = swAtt.GetEntityState(swAssociatedEntityStates_e.swIsEntityAmbiguous) And False = swAtt.GetEntityState(swAssociatedEntityStates_e.swIsEntityDeleted) Then
swParamName = swAtt.GetParameter(AttLenDimName)
swParamValue = swAtt.GetParameter(AttLenValueName)
Debug.Print("Attribute " & swParamName.GetStringValue & " found.")
Debug.Print(" Value = " & swParamValue.GetDoubleValue)
Else
Debug.Print(" Attribute found, but problems exist.")
End If
Else
Debug.Print(" Attribute not found.")
End If
End Sub
''' <summary>
''' The SldWorks swApp variable is pre-assigned for you.
''' </summary>
Public swApp As SldWorks
End Class