Hide Table of Contents

Get ID of Active Configuration or Current Drawing Sheet Example (VB.NET)

This example shows how to get the name and ID of the active configuration or the current drawing sheet.

A unique ID is assigned to each configuration and drawing. This ID does not change when the name of the configuration or drawing sheet is changed.

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

' Preconditions: Part, assembly, or drawing document is open.

'

' Postconditions: Either the active configuration's name or

'       the current sheet's name is changed to "Test"; however,

'       its ID remains unchanged.

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

Imports SolidWorks.Interop.sldworks

Imports SolidWorks.Interop.swconst

Imports System

Imports System.Diagnostics

 

Partial Class SolidWorksMacro

 

    Public Sub main()

 

        Dim swModel As ModelDoc2

        Dim swConfig As Configuration

        Dim swDrawingDoc As DrawingDoc

        Dim swSheet As Sheet

        Dim nDocType As Long

 

        swModel = swApp.ActiveDoc

 

        ' Get type of model document

        If swModel.GetType = 1 Then

            nDocType = swDocumentTypes_e.swDocPART

        ElseIf swModel.GetType = 2 Then

            nDocType = swDocumentTypes_e.swDocASSEMBLY

        ElseIf swModel.GetType = 3 Then

            nDocType = swDocumentTypes_e.swDocDRAWING

        Else

            ' Not a SolidWorks model document,

            ' so exit macro

            Exit Sub

        End If

 

        ' If a part or assembly document,

        ' then get the name of it and its ID

        If nDocType <> swDocumentTypes_e.swDocDRAWING Then

            swConfig = swModel.GetActiveConfiguration

            If Not swConfig Is Nothing Then

                Debug.Print("Active configuration's name = " & swConfig.Name & ", ID = " & swConfig.GetID)

                ' Change the active configuration's name

                swConfig.Name = "Test"

                ' Test to see if the ID remains the same

                ' after changing the name of the configuration

                Debug.Print("Active configuration's new name = " & swConfig.Name & ", ID = " & swConfig.GetID)

            End If

            Exit Sub

        End If

 

        ' A drawing sheet must be active,

        ' so get its name and ID

        swDrawingDoc = swModel

        swSheet = swDrawingDoc.GetCurrentSheet

        If Not swSheet Is Nothing Then

            Debug.Print("Current sheet's name = " & swSheet.GetName & ", ID = " & swSheet.GetID)

            ' Change current sheet's name

            swSheet.SetName("Test")

            ' Test to see if the ID remains the same

            ' after changing the name of the sheet

            Debug.Print("Current sheet's new name = " & swSheet.GetName & ", ID = " & swSheet.GetID)

        End If

 

    End Sub

 

    ''' <summary>

    ''' The SldWorks swApp variable is pre-assigned for you.

    ''' </summary>

    Public swApp As SldWorks

 

End Class



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Get ID of Active Configuration or Current Drawing Sheet Example (VB.NET)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2010 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.