Description

This macro converts an active SolidWorks assembly into a part file that contains only the exterior components. This feature is useful for reducing the complexity of the assembly when sharing with external stakeholders or for performance improvements in visualization and analysis.

System Requirements

• SOLIDWORKS Version: SOLIDWORKS 2014 or newer
• Operating System: Windows 7 or later

Prerequisites

The following conditions must be satisfied for the macro to function as intended:

• An assembly document (.SLDASM) must be currently open and the frontmost document in SOLIDWORKS.
• The active assembly document must contain at least one part component to make the operation meaningful.

Results

• The macro successfully takes the active assembly and saves it as a new part file (.SLDPRT) that contains only exterior geometry.
• The part file is automatically saved in the same directory as the original assembly file using the same file name base, except with the extension .SLDPRT.
• The original assembly document remains unchanged.

Steps to Set Up the Macro

To deploy the SOLIDWORKS macro to save assembly as part utility, you must follow these simple steps:

Prepare SolidWorks

• Open SolidWorks and load the assembly document you wish to modify.
• Your assembly must contain at least one part component.

Configure and Run the Macro

• Open the SolidWorks VBA editor by pressing (Alt + F11) from within SolidWorks.
• Add a new module, and copy the VBA macro code provided below into the module you added. The module serves as the permanent destination for the code, ensuring the utility is saved within SOLIDWORKS for repeated, quick access.
• Next, execute the macro in SolidWorks by navigating to Tools > Macro > Run, and select the file you saved.

Outcome of Using the Macro

• The macro will automatically save the active document as a new part file containing only the exterior parts.
• The automation handles all the complex API settings for Save As Part simplification, ensuring that every time it is executed, in the same way, and the document preserves the history as a part file.
• The original assembly will remain unchanged.

VBA Macro Code

' Disclaimer:
' The code provided should be used at your own risk.  
' Blue Byte Systems Inc. assumes no responsibility for any issues or damages that may arise from using or modifying this code.  
' For more information, visit [Blue Byte Systems Inc.](https://bluebyte.biz).

Option Explicit

' SolidWorks application and document variables
Dim swApp As SldWorks.SldWorks                    ' SolidWorks application object
Dim swModel As SldWorks.ModelDoc2                 ' Active SolidWorks document object
Dim swModelDocExt As SldWorks.ModelDocExtension   ' Extension object for advanced file operations
Dim FilePath As String                            ' Full file path of the current document
Dim PathSize As Long                              ' Length of the file path
Dim PathNoExtension As String                     ' File path without extension
Dim NewFilePath As String                         ' File path for the new part file
Dim nErrors As Long                               ' Counter for errors during the save operation
Dim nWarnings As Long                             ' Counter for warnings during the save operation

' Main subroutine
Sub main()
    ' Initialize SolidWorks application and get the active document
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc

    ' Check if a document is open
    If swModel Is Nothing Then
        MsgBox "No active document found. Please open a file."
        Exit Sub
    End If

    ' Get the ModelDocExtension object for advanced operations
    Set swModelDocExt = swModel.Extension

    ' Extract the file path and prepare the new file path
    FilePath = swModel.GetPathName                     ' Get the full file path of the active document
    PathSize = Strings.Len(FilePath)                  ' Get the length of the file path
    PathNoExtension = Strings.Left(FilePath, PathSize - 6) ' Remove the last 6 characters (e.g., ".SLDASM")
    NewFilePath = PathNoExtension & "SLDPRT"          ' Append "SLDPRT" to create the new file path

    ' Set options to save only the exterior components
    swApp.SetUserPreferenceIntegerValue swSaveAssemblyAsPartOptions, swSaveAsmAsPart_ExteriorComponents

    ' Save the assembly as a new part file
    swModelDocExt.SaveAs NewFilePath, swSaveAsCurrentVersion, swSaveAsOptions_Silent, Nothing, nErrors, nWarnings

    ' Check for errors and warnings during the save operation
    If nErrors = 0 And nWarnings = 0 Then
        ' Success: Notify the user that the save operation was successful
        MsgBox "Assembly saved as part file successfully at: " & NewFilePath
    Else
        ' Failure: Notify the user about errors and warnings
        MsgBox "Failed to save assembly as part file. Errors: " & nErrors & ", Warnings: " & nWarnings
    End If
End Sub

Macro

You can download the macro from here.

Customization and Advanced Solutions by Experts

To get started with customizing this macro or to create any other fully custom solutions for your engineering projects, reach out to our team of engineers today!