Get Editing Status of Features Example (VBA)

This example shows how to get the editing status of one or more features.

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

' Preconditions:

' 1. Open:

' <SolidWorks_install_dir>\samples\tutorial\introtosw\pressure_plate.sldprt

' 2. Insert a breakpoint in your macro at this line:

' retVal = swModelDocExt.SelectByID2

' ("Sketch2", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)

' 3. Run the macro (F5) and then step into the code using

'    the debugger (F8) after execution stops at the breakpoint.

' 4. Examine the results displayed in the Immediate window and

'    FeatureManager design tree while stepping through the

'    remaining code.

'

' Postconditions: None

'

' NOTE: Because this document is used by a SolidWorks

'       online tutorial, do not save any changes when

'       closing the document.

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

Option Explicit

 

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swFeatMgr As SldWorks.FeatureManager

Dim swSelMgr As SldWorks.SelectionMgr

Dim swModelDocExt As SldWorks.ModelDocExtension

Dim varFeat  As Variant

Dim editStatus As Long

Dim retVal As Boolean

Dim i As Long

Dim featName As String

 

Sub main()

 

Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swFeatMgr = swModel.FeatureManager

Set swSelMgr = swModel.SelectionManager

Set swModelDocExt = swModel.Extension

 

' Traverse through the FeatureManager design tree

' to get the editing status of all features

' Change the editing status of a sketch and feature

' during feature traversal

varFeat = swFeatMgr.GetFeatures(True)

editStatus = swFeature_NonEditable

For i = LBound(varFeat) To UBound(varFeat)

    Dim swFeat As SldWorks.Feature

    Set swFeat = varFeat(i)

    featName = swFeat.Name

    Select Case (featName)

        Case "Sketch2"

            ' Select and edit a sketch

            retVal = swModelDocExt.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)

            swModel.EditSketch

        Case "Extrude3"

            ' Close the open sketch

            swModel.InsertSketch2 True

        Case "Cut-Extrude2"

            ' Select and edit a feature

            retVal = swModelDocExt.SelectByID2("Cut-Extrude2", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)

            swModel.FeatEdit

    End Select

    ' Get the editing status of the current feature

    editStatus = swFeat.GetEditStatus

    Select Case (editStatus)

        Case 0

            Debug.Print (swFeat.Name & " can be edited.")

        Case 1

            Debug.Print (swFeat.Name & " cannot currently be edited.")

        Case 2

            Debug.Print (swFeat.Name & " is already being edited.")

    End Select

    Set swFeat = Nothing

Next i

 

' End feature editing

swModel.InsertSketch2 True

 

End Sub