SOLIDWORKS Macro to Delete Unused Sketches and Reference Geometry

Description

• Finds planes, axes, points, coordinate systems and sketches that nothing depends on.
• Lists them and deletes them after you confirm.
• The Front, Top and Right planes are always kept.

System Requirements

• SOLIDWORKS Version: SOLIDWORKS 2014 or newer
• Operating System: Windows 10 or later

Pre-Requisites

• The active document must be a part or an assembly.

Results

• Unused features are removed from the FeatureManager design tree.
• Use Undo if you need any of them back.

Steps to Set Up the Macro

1. Open SOLIDWORKS and the document described in the pre-requisites.

2. Create the macro

• Go to Tools > Macro > New, give the .swp file a name and save it. The VBA editor opens.
• Replace everything in the module with the code below.

3. Run the macro

• Press F5 in the VBA editor, or use Tools > Macro > Run.
• For daily use, assign it to a toolbar button or keyboard shortcut via Tools > Customize.

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 https://bluebyte.biz
' Reviewed and updated by Blue Byte Systems Inc.

Option Explicit

' Finds unused reference geometry and sketches (features with no children)
' in the active part or assembly, lists them and deletes them after confirmation.
' Types checked: planes, axes, points, coordinate systems, 2D and 3D sketches.
' The three default planes (Front, Top, Right) are always kept.

Sub main()
    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swFeat As SldWorks.Feature
    Dim vChildren As Variant
    Dim found As New Collection
    Dim label As String
    Dim listText As String
    Dim planeCount As Long
    Dim i As Long

    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc

    If swModel Is Nothing Then
        MsgBox "Open a part or assembly before running this macro.", vbExclamation
        Exit Sub
    End If
    If swModel.GetType = swDocDRAWING Then
        MsgBox "This macro works on parts and assemblies.", vbExclamation
        Exit Sub
    End If

    Set swFeat = swModel.FirstFeature
    Do While Not swFeat Is Nothing
        label = ""
        Select Case swFeat.GetTypeName2
            Case "RefPlane"
                planeCount = planeCount + 1
                If planeCount > 3 Then label = "Plane"     ' skip Front, Top, Right
            Case "RefAxis":          label = "Axis"
            Case "RefPoint":         label = "Point"
            Case "CoordSys":         label = "Coordinate system"
            Case "ProfileFeature":   label = "Sketch"
            Case "3DProfileFeature": label = "3D sketch"
        End Select

        If label <> "" Then
            vChildren = swFeat.GetChildren
            If IsEmpty(vChildren) Then
                found.Add swFeat
                If found.Count <= 25 Then listText = listText & vbCrLf & swFeat.Name & "  (" & label & ")"
            End If
        End If
        Set swFeat = swFeat.GetNextFeature
    Loop

    If found.Count = 0 Then
        MsgBox "No unused features found.", vbInformation
        Exit Sub
    End If
    If found.Count > 25 Then listText = listText & vbCrLf & "... and " & (found.Count - 25) & " more"

    If MsgBox(found.Count & " unused feature(s) found:" & vbCrLf & listText & vbCrLf & vbCrLf & _
              "Delete them?", vbYesNo + vbQuestion) <> vbYes Then Exit Sub

    swModel.ClearSelection2 True
    For i = 1 To found.Count
        found(i).Select2 True, -1
    Next
    swModel.Extension.DeleteSelection2 swDelete_Absorbed
    swModel.ForceRebuild3 False

    MsgBox found.Count & " feature(s) deleted. Use Undo if you need any back.", vbInformation
End Sub

Code Review Notes

We reviewed this macro before publishing it here. Changes from the original version:

• The original needed a separate UserForm that was not published with the code. It now runs from a single module.
• Works in assemblies as well as parts, and the default planes are protected.

Need to customize the macro?

Contact us and we will adapt this macro to your workflow, or build a complete SOLIDWORKS or PDM automation for your team.