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Get Mirror Solid Feature Data Example (VB.NET)

This example shows how to get data for a mirror solid feature.

'------------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified part document to open exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens the specified part document.
' 2. Selects a plane and solid body.
' 3. Mirrors the solid body.
' 4. Gets the mirror solid feature and some of its data.
' 5. Prints to the Immediate window some mirror solid feature data.
' 6. Examine the Immediate window, FeatureManager design tree, and graphics
'    area.
'
' NOTE: Because the part is used elsewhere, do not save changes.
'-----------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
 
Partial Class SolidWorksMacro
 
    Public Sub main()
 
        Dim swModel As ModelDoc2
        Dim swModelDocExt As ModelDocExtension
        Dim swFeatureManager As FeatureManager
        Dim swFeature As Feature
        Dim swMirrorSolidFeatureData As MirrorSolidFeatureData
        Dim swBody As Body2
        Dim swSelectionMgr As SelectionMgr
        Dim swSelData As SelectData
        Dim status As Boolean
        Dim errors As Integer
        Dim warnings As Integer
        Dim fileName As String
        Dim i As Integer
        Dim bodies() As Object
 
        'Open part
        fileName = "C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\multibody\multi_inter.sldprt"
        swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
 
        'Select plane and solid body
        swModelDocExt = swModel.Extension
        status = swModelDocExt.SelectByID2("Top""PLANE", 0, 0, 0, True, 0, Nothing, 0)
        status = swModelDocExt.SelectByID2("Extrude-Thin1""SOLIDBODY", 0, 0, 0, True, 0, Nothing, 0)
        swModel.ClearSelection2(True)
        status = swModelDocExt.SelectByID2("Top""PLANE", 0, 0, 0, False, 2, Nothing, 0)
        status = swModelDocExt.SelectByID2("Extrude-Thin1""SOLIDBODY", 0, 0, 0, True, 256, Nothing, 0)
 
        'Insert mirror solid feature
        swFeatureManager = swModel.FeatureManager
        swFeature = swFeatureManager.InsertMirrorFeature2(TrueFalseFalseFalse, swFeatureScope_e.swFeatureScope_AllBodies)
 
        'Get mirror solid feature and some of its data
        swMirrorSolidFeatureData = swFeature.GetDefinition
        Debug.Print("  " & swFeature.Name)
        Debug.Print("    Number of bodies               = " & swMirrorSolidFeatureData.GetPatternBodyCount)
        Debug.Print("    Merged bodies                  = " & swMirrorSolidFeatureData.Merge)
        Debug.Print("    Knit surfaces                  = " & swMirrorSolidFeatureData.KnitSurface)
 
        'Roll back to get to the bodies
        status = swMirrorSolidFeatureData.AccessSelections(swModel, Nothing)
        swSelectionMgr = swModel.SelectionManager
        swSelData = swSelectionMgr.CreateSelectData
        bodies = swMirrorSolidFeatureData.PatternBodyArray
        For i = 0 To UBound(bodies)
            swBody = bodies(i)
            status = swBody.Select(True, 0)
            Debug.Print("    Body " & i + 1 & "'s type (solid body = 0) = " & swBody.GetType)
        Next i
 
        'Release selection access
        swMirrorSolidFeatureData.ReleaseSelectionAccess()
 
    End Sub
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
 
 
End Class


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