Get Editing Status of Features Example (VB.NET)
This example shows how to get the editing status of one or more features.
'------------------------------------------------------------------------
' Preconditions
' 1. Open install_dir\samples\tutorial\introtosw\pressure_plate.sldprt.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. At Stop, examine the the Immediate window, graphics area, and
' FeatureManager design tree.
' 2. Press F5.
' 3. Examine the Immediate window again.
'
' NOTE: Because this document is used elsewhere, do not save changes.
'-------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System
Imports System.Diagnostics
Partial Class SolidWorksMacro
Public Sub main()
Dim swModel As ModelDoc2
Dim swFeatMgr As FeatureManager
Dim swSelMgr As SelectionMgr
Dim swModelDocExt As ModelDocExtension
Dim varFeat As Object
Dim editStatus As Long
Dim retVal As Boolean
Dim i As Long
Dim featName As String
swModel = swApp.ActiveDoc
swFeatMgr = swModel.FeatureManager
swSelMgr = swModel.SelectionManager
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 = swFeatureEditStatus_e.swFeature_NonEditable
For i = LBound(varFeat) To UBound(varFeat)
Dim swFeat As Feature
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()
Stop
' Examine the Immediate window, graphics area, and FeatureManager design tree
' All of the features beneath Extrude1 cannot be edited because
' Extrude2's Sketch2 is in edit mode
' Press F5
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
swFeat = Nothing
Next i
' End feature editing
swModel.InsertSketch2(True)
End Sub
''' <summary>
''' The SldWorks swApp variable is pre-assigned for you.
''' </summary>
Public swApp As SldWorks
End Class