Function AutoMateRepair( _
   ByRef ProcessedMates As System.Object, _
   ByRef FailedMates As System.Object _
) As System.Integer

Dim instance As IAssemblyDoc
Dim ProcessedMates As System.Object
Dim FailedMates As System.Object
Dim value As System.Integer
 
value = instance.AutoMateRepair(ProcessedMates, FailedMates)

System.int AutoMateRepair( 
   out System.object ProcessedMates,
   out System.object FailedMates
)

System.int AutoMateRepair( 
&   [Out] System.Object^ ProcessedMates,
&   [Out] System.Object^ FailedMates
) 

Parameters

ProcessedMates

Array of successfully repaired IMate2s

FailedMates

Array of failed IMate2s

Return Value

'VBA

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

' Preconditions:

' 1. Open the Immediate window.

' 2. Ensure that c:\temp and the specified templates exist.

'

' Postconditions:

' 1. When the macro stops, inspect the FeatureManager design tree.

'    Observe that two Cylinder_225 components, two planes, and two mates are added to the assembly.

' 2. In the FeatureManager design tree delete PLANE2.

'    Observe that Cylinder_225<1> and Coincident2 are red, indicating a mate error has occurred.

' 3. In the user interface add a reference plane that is 1 mm from the Front Plane.

' 4. In the FeatureManager design tree select the Mates folder.

' 5. Press F5 to autorepair the broken mate.

'    The Immediate window shows one repaired mate.

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

Dim swApp As SldWorks.SldWorks

Dim Part As SldWorks.ModelDoc2

Dim boolstatus As Boolean

Dim longstatus As Long, longwarnings As Long

Option Explicit

Sub main()

    Set swApp = Application.SldWorks

    Dim swSheetWidth As Double

    swSheetWidth = 0

    Dim swSheetHeight As Double

    swSheetHeight = 0

    Set Part = swApp.NewDocument("c:\temp\Part.prtdot", 0, swSheetWidth, swSheetHeight)

    Dim swPart As SldWorks.PartDoc

    Set swPart = Part

    swApp.ActivateDoc2 "Part1", False, longstatus

    Set Part = swApp.ActiveDoc

    Dim myModelView As SldWorks.ModelView

    Set myModelView = Part.ActiveView

    myModelView.FrameState = swWindowState_e.swWindowMaximized

    Part.SketchManager.InsertSketch True

    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -0.068513658157061, 4.03895355082156E-02, 8.71366929740688E-03, False, 0, Nothing, 0)

    Part.ClearSelection2 True

    Dim skSegment As Object

    Set skSegment = Part.SketchManager.CreateCircle(0#, 0#, 0#, 0.045995, 0.021666, 0#)

    Part.ShowNamedView2 "*Trimetric", 8

    Part.ViewZoomtofit2

    Dim myFeature As SldWorks.Feature

    Set myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, False, 0, 0, 0.225, 0.01, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, True, True, True, 0, 0, False)

    Part.SelectionManager.EnableContourSelection = False

    ' Save As

    longstatus = Part.SaveAs3("c:\temp\Cylinder_225.SLDPRT", 0, 0)

    swSheetWidth = 0

    swSheetHeight = 0

    Set Part = swApp.NewDocument("c:\temp\Assembly.asmdot", 0, swSheetWidth, swSheetHeight)

    Dim swAssembly As SldWorks.AssemblyDoc

    Set swAssembly = Part

    swApp.ActivateDoc2 "Assem3", False, longstatus

    Set Part = swApp.ActiveDoc

    Set myModelView = Part.ActiveView

    myModelView.FrameState = swWindowState_e.swWindowMaximized

    ' Insert Component

    Dim AssemblyTitle As String

    AssemblyTitle = Part.GetTitle

    Dim tmpObj As SldWorks.ModelDoc2

    Dim errors As Long

    Set tmpObj = swApp.OpenDoc6("c:\temp\Cylinder_225.SLDPRT", 1, 32, "", errors, longwarnings)

    Set Part = swApp.ActivateDoc3(AssemblyTitle, True, 0, errors)

    Dim swInsertedComponent As SldWorks.Component2

    Set swInsertedComponent = Part.AddComponent5("c:\temp\Cylinder_225.SLDPRT", 0, "", False, "", 0.721748083354866, 0.92923566513213, 1.36775956940221)

    swApp.CloseDoc "c:\temp\Cylinder_225.SLDPRT"

    boolstatus = Part.Extension.SelectByID2("Cylinder_225-1", "COMPONENT", 0, 0, 0, False, 0, Nothing, 0)

    Part.UnfixComponent

    ' Create PLANE1 and PLANE2

    boolstatus = Part.SetUserPreferenceToggle(swUserPreferenceToggle_e.swDisplayPlanes, True)

    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)

    Dim myRefPlane As SldWorks.RefPlane

    Set myRefPlane = Part.FeatureManager.InsertRefPlane(8, 0.1, 0, 0, 0, 0)

    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)

    Set myRefPlane = Part.FeatureManager.InsertRefPlane(8, 0.001, 0, 0, 0, 0)

    Part.ClearSelection2 True

    ' Insert Component

    AssemblyTitle = Part.GetTitle

    Set tmpObj = swApp.OpenDoc6("c:\temp\Cylinder_225.SLDPRT", 1, 32, "", errors, longwarnings)

    Set Part = swApp.ActivateDoc3(AssemblyTitle, True, 0, errors)

    Set swInsertedComponent = Part.AddComponent5("c:\temp\Cylinder_225.SLDPRT", 0, "", False, "", -9.24876597127877E-02, 5.65812429995276E-02, 0.22909678472206)

    swApp.CloseDoc "c:\temp\Cylinder_225.SLDPRT"

    Part.ClearSelection2 True

    boolstatus = Part.Extension.SelectByID2("PLANE1", "PLANE", 0.012624285665936, 0.154967158689601, 0.112309569516221, True, 1, Nothing, 0)

    boolstatus = Part.Extension.SelectByRay(-0.076247080467482, 0.103507691590153, 0.115945777078347, -0.283810108456217, -0.958610200111282, 2.27663475480263E-02, 2.30409955137483E-03, 1, True, 1, 0)

    ' Create CoincidentMateFeatureData

    Dim MateData As SldWorks.CoincidentMateFeatureData

    Set MateData = Part.CreateMateData(0)

    ' Set the Entities To Mate

    Dim EntitiesToMate(1) As Object

    Set EntitiesToMate(0) = Part.SelectionManager.GetSelectedObject6(1, -1)

    Set EntitiesToMate(1) = Part.SelectionManager.GetSelectedObject6(2, -1)

    Dim EntitiesToMateVar As Variant

    EntitiesToMateVar = EntitiesToMate

    MateData.EntitiesToMate = (EntitiesToMateVar)

    ' Set the Mate Alignment

    MateData.MateAlignment = 1

    ' Create the mate

    Dim MateFeature As SldWorks.Feature

    Set MateFeature = Part.CreateMate(MateData)

    Part.ClearSelection2 True

    Part.EditRebuild3

    Part.ClearSelection2 True

    boolstatus = Part.Extension.SelectByID2("PLANE2", "PLANE", -0.051265823820458, 0.210240836185798, -8.14719342065839E-02, True, 1, Nothing, 0)

    boolstatus = Part.Extension.SelectByRay(0.767058330396253, 0.909200270895155, 1.48052500817425, -0.400036026779312, -0.515038074910024, -0.758094294050284, 1.12587739183236E-02, 1, True, 0, 0)

    ' Create CoincidentMateFeatureData

    Set MateData = Part.CreateMateData(0)

    ' Set the Entities To Mate

    Set EntitiesToMate(0) = Part.SelectionManager.GetSelectedObject6(1, -1)

    Set EntitiesToMate(1) = Part.SelectionManager.GetSelectedObject6(2, -1)

    EntitiesToMateVar = EntitiesToMate

    MateData.EntitiesToMate = (EntitiesToMateVar)

    ' Set the Mate Alignment

    MateData.MateAlignment = 1

    ' Create the mate

    Set MateFeature = Part.CreateMate(MateData)

    Part.ClearSelection2 True

    Part.EditRebuild3

    Part.ViewZoomtofit2

    Stop  ' Delete Plane2; create a new plane that is 1mm from the Front Plane; select the Mates folder in the FeatureManager design tree; then press F5 to repair the broken mate

    Dim swModel As SldWorks.ModelDoc2

    Dim cnt As Long

    Set swModel = swApp.ActiveDoc

    Dim swAsm As SldWorks.AssemblyDoc

    Set swAsm = swModel

    Dim failedMates As Variant

    Dim ProcessedMates As Variant

    Dim lStatus As Long

    lStatus = swAsm.AutoMateRepair(ProcessedMates, failedMates)

    Debug.Print "Number of Processed Mates is " & UBound(ProcessedMates) + 1 & ":"

    For cnt = 0 To UBound(ProcessedMates)

    Debug.Print ProcessedMates(cnt).Name

    Next

    Debug.Print vbNewLine

    Debug.Print "Number of failed Mates is " & UBound(failedMates) + 1 & ":"

    For cnt = 0 To UBound(failedMates)

    Debug.Print failedMates(cnt).Name

    Next

End Sub

Before calling this method you must:

• ensure that the entities needed to repair the broken mates are present in the assembly

    - and -

• select the Mates folder in the FeatureManager design tree.