Journal for Engraving

Hello All,
Below journal creates the Engraving on the part body by extracting details from part attributes such as Description, Part number (removed the last 5 characters of the string from the part number for my requirement)& Weight.

' NX 12.0.1.7
' Journal created by Balaji_Sampath03 on Tue Jul 21 20:07:10 2020 India Standard Time
'**************************************************************************************
'This Journal creates the Engraving on the NX part with attribute info such as
'1> Description
'2> Part Number (last 4 characters of the string from part number is removed) and
'3> Weight
'This Journal does not have any exception to catch any errors
'Has option to invert the direction of the Offset curve before the final extrude option
'***************************************************************************************
Option Strict Off
Imports System
Imports System.Collections.Generic
Imports NXOpen
Imports NXOpen.UI
Imports NXOpen.UF

Module NXJournal

Dim theUfSession As UFSession = UFSession.GetUFSession()
Dim theSession As NXOpen.Session = NXOpen.Session.GetSession()
Dim workPart As NXOpen.Part = theSession.Parts.Work
Dim displayPart As NXOpen.Part = theSession.Parts.Display
Dim lw As ListingWindow = theSession.ListingWindow
Dim theUI As UI = UI.GetUI()

Sub Main (ByVal args() As String)

Dim attDesc As String = Nothing
Dim attPartNum As String = Nothing
Dim attWeight As Double = Nothing
Dim attributeInfo As NXObject.AttributeInformation

' -------------------
' GET USER ATTRIBUTES
' -------------------

If workPart.HasUserAttribute("DESCRIPTION", NXObject.AttributeType.Any, -1) Then
attributeInfo = workPart.GetUserAttribute("Description", NXObject.AttributeType.String, -1)
attDesc = attributeInfo.StringValue
Else
lw.WriteLine("Attribute 'DESCRIPTION' is not present")
End If

If workPart.HasUserAttribute("Weight", NXObject.AttributeType.Any, -1) Then
Dim aInfo As NXObject.AttributeInformation
aInfo = workPart.GetUserAttribute("Weight", NXObject.AttributeType.Any, -1)
attWeight = aInfo.StringValue
Else
lw.WriteLine("Attribute 'Weight' is not present")
attWeight = " "
End If

attPartnum = workPart.Name

' -----------------------------------------------------------------
' CREATE FEATURE GROUP "ENGRAVE TEXT" AND MAKE FEATURE GROUP ACTIVE
' -----------------------------------------------------------------

Dim markId1 As NXOpen.Session.UndoMarkId = Nothing
markId1 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Visible, "Feature Groups")

Dim activatefeaturegroupwithrollback1 As Boolean = Nothing
activatefeaturegroupwithrollback1 = theSession.Preferences.Modeling.ActivateFeatureGroupWithRollback

Dim featuresToGroup As Tag() = Nothing
Dim theFeatureGroupTag As Tag = Nothing
theUfSession.Modl.CreateSetOfFeature("ENGRAVE TEXT", featuresToGroup, 0, 1, theFeatureGroupTag)

For Each myFeature As Features.Feature In workPart.Features
If TypeOf (myFeature) Is NXOpen.Features.FeatureGroup Then
If myFeature.FeatureType = "FSET" And myFeature.Name = "ENGRAVE TEXT" Then
myFeature.MakeCurrentFeature()
myFeature.SetGroupActive(True)
End If
End If
Next

' ---------------------------------------------------
' SET PARAMETERS FOR CURVE SEL AND FACE OFFSET METHOD
' ---------------------------------------------------

Dim nullNXOpen_Features_Feature As NXOpen.Features.Feature = Nothing

Dim aOCSBuilder1 As NXOpen.Features.AOCSBuilder = Nothing
aOCSBuilder1 = workPart.Features.CreateAocsBuilder(nullNXOpen_Features_Feature)

Dim lawBuilder1 As NXOpen.GeometricUtilities.LawBuilder = Nothing
lawBuilder1 = aOCSBuilder1.Law

Dim alongSpineBuilder1 As NXOpen.GeometricUtilities.AlongSpineBuilder = Nothing
alongSpineBuilder1 = lawBuilder1.AlongSpineData

Dim unit1 As NXOpen.Unit = Nothing
unit1 = aOCSBuilder1.FilletRadius.Units

Dim curveFitData1 As NXOpen.GeometricUtilities.CurveFitData = Nothing
curveFitData1 = aOCSBuilder1.CurveFitData

Dim nullNXOpen_ScCollector As NXOpen.ScCollector = Nothing

aOCSBuilder1.FaceCollector = nullNXOpen_ScCollector

aOCSBuilder1.OffsetDistType = NXOpen.Features.AOCSBuilder.OffsetDistanceType.Constant
aOCSBuilder1.OffsetDirectionOption = NXOpen.Features.AOCSBuilder.OffsetDirection.NormalToCurve
aOCSBuilder1.OffsetMode = NXOpen.Features.AOCSBuilder.OffsetType.Tangential
aOCSBuilder1.TrimMethod = NXOpen.Features.AOCSBuilder.Trim.WithinSection
aOCSBuilder1.ExtendMethod = NXOpen.Features.AOCSBuilder.Extend.WithinSection
aOCSBuilder1.TrimToFaceEdgesOption = False
aOCSBuilder1.ExtendToFaceOption = NXOpen.Features.AOCSBuilder.ExtendToFace.Boundary
aOCSBuilder1.RemoveSelfIntersections = True
aOCSBuilder1.AssociativeOutputOption = True
aOCSBuilder1.LawStringFlip = False
aOCSBuilder1.SplitCurveOption = True
aOCSBuilder1.OffsetDirectionOption = NXOpen.Features.AOCSBuilder.OffsetDirection.NormalToCurve

aOCSBuilder1.FilletOption = NXOpen.Features.AOCSBuilder.FilletOptions.NoFillet
aOCSBuilder1.CurveOffsetType = NXOpen.Features.AOCSBuilder.CurveOffsetTypes.Value

Dim nullNXOpen_Point As NXOpen.Point = Nothing

aOCSBuilder1.ThroughPoint = nullNXOpen_Point

Dim objectList1 As NXOpen.ObjectList = Nothing
objectList1 = alongSpineBuilder1.SpinePointList
objectList1.Clear(NXOpen.ObjectList.DeleteOption.Delete)

Dim origin1 As NXOpen.Point3d = New NXOpen.Point3d(0.0, 0.0, 0.0)
Dim vector1 As NXOpen.Vector3d = New NXOpen.Vector3d(1.0, 0.0, 0.0)
Dim direction1 As NXOpen.Direction = Nothing
direction1 = workPart.Directions.CreateDirection(origin1, vector1, NXOpen.SmartObject.UpdateOption.WithinModeling)

aOCSBuilder1.ProjectPlaneNormal = direction1

Dim section1 As NXOpen.Section = Nothing
section1 = workPart.Sections.CreateSection(0.0094999999999999998, 0.01, 0.5)

Dim nullNXOpen_Section As NXOpen.Section = Nothing

Dim expressionSectionSet1 As NXOpen.ExpressionSectionSet = Nothing
expressionSectionSet1 = workPart.CreateExpressionSectionSet(nullNXOpen_Section, "2", "Length", 0)

expressionSectionSet1.ItemFlipFlag = True
aOCSBuilder1.Offsets.Append(expressionSectionSet1)

section1.SetAllowedEntityTypes(NXOpen.Section.AllowTypes.OnlyCurves)

' ------------------------
' SELECT CURVE TO OFFSET
' ------------------------

Dim pickEdge As Edge

If SelectEdge("Select Edge", pickEdge) = Selection.Response.Cancel Then
Return
End If

Dim edges1(0) As NXOpen.Edge
edges1(0) = pickEdge

Dim edgeDumbRule1 As NXOpen.EdgeDumbRule = Nothing
edgeDumbRule1 = workPart.ScRuleFactory.CreateRuleEdgeDumb(edges1)

section1.AllowSelfIntersection(False)

Dim rules1(0) As NXOpen.SelectionIntentRule
rules1(0) = edgeDumbRule1
Dim nullNXOpen_NXObject As NXOpen.NXObject = Nothing

Dim helpPoint1 As NXOpen.Point3d = New NXOpen.Point3d(-51.890018880214939, -40.000000000000043, 10.0)
section1.AddToSection(rules1, pickEdge, nullNXOpen_NXObject, nullNXOpen_NXObject, helpPoint1, NXOpen.Section.Mode.Create, False)

expressionSectionSet1.Section = section1

' ----------------------
' SELECT FACE FOR OFFSET
' ----------------------

Dim scCollector1 As NXOpen.ScCollector = Nothing
scCollector1 = workPart.ScCollectors.CreateCollector()

Dim pickFace As Face
SelectAFace("select a face", pickFace)

Dim faces1(0) As NXOpen.Face
faces1(0) = pickFace

Dim faceDumbRule1 As NXOpen.FaceDumbRule = Nothing
faceDumbRule1 = workPart.ScRuleFactory.CreateRuleFaceDumb(faces1)
Dim rules2(0) As NXOpen.SelectionIntentRule
rules2(0) = faceDumbRule1
scCollector1.ReplaceRules(rules2, False)

aOCSBuilder1.FaceCollector = scCollector1
aOCSBuilder1.UpdateFaces()

Dim feature1 As NXOpen.Features.Feature = Nothing
feature1 = aOCSBuilder1.CommitFeature()
aOCSBuilder1.Destroy()

' -------------------------------------------
' INSERT TEXT 1 AND SEL OFFSET CURVE FOR TEXT
' -------------------------------------------

Dim nullNXOpen_Features_Text As NXOpen.Features.Text = Nothing

Dim textBuilder1 As NXOpen.Features.TextBuilder = Nothing
textBuilder1 = workPart.Features.CreateTextBuilder(nullNXOpen_Features_Text)

textBuilder1.TextString = ("WEIGHT: " & attWeight.ToString("0.00") & " kg")
textBuilder1.FrameOnPath.AnchorPosition.Expression.RightHandSide = "50"
textBuilder1.Type = NXOpen.Features.TextBuilder.Types.OnFace
textBuilder1.PlanarFrame.Shear.RightHandSide = "0"
textBuilder1.FrameOnPath.AnchorLocation = NXOpen.GeometricUtilities.FrameOnPathBuilder.AnchorLocationType.Left
textBuilder1.FrameOnPath.AnchorPosition.Expression.RightHandSide = "5"
textBuilder1.FrameOnPath.Height.RightHandSide = "5"
textBuilder1.PrintMarkThickness.RightHandSide = "1"
textBuilder1.FrameOnPath.WScale = 100.0
textBuilder1.FrameOnPath.Offset.RightHandSide = "0"
textBuilder1.SelectFont("Arial", NXOpen.Features.TextBuilder.ScriptOptions.Western)

Dim boundaryFaces1(-1) As NXOpen.Face
Dim faceTangentRule1 As NXOpen.FaceTangentRule = Nothing
faceTangentRule1 = workPart.ScRuleFactory.CreateRuleFaceTangent(pickFace, boundaryFaces1, 0.5)

Dim rules3(0) As NXOpen.SelectionIntentRule
rules3(0) = faceTangentRule1
textBuilder1.PlacementFaces.ReplaceRules(rules3, False)

textBuilder1.OnFacePlacementProfile.SetAllowedEntityTypes(NXOpen.Section.AllowTypes.OnlyCurves)

Dim features1(0) As NXOpen.Features.Feature
Dim aOCS1 As NXOpen.Features.AOCS = CType(feature1, NXOpen.Features.AOCS)

features1(0) = aOCS1
Dim line1 As NXOpen.Line = CType(aOCS1.FindObject("CURVE 1"), NXOpen.Line)

Dim nullNXOpen_Curve As NXOpen.Curve = Nothing

Dim curveFeatureTangentRule1 As NXOpen.CurveFeatureTangentRule = Nothing
curveFeatureTangentRule1 = workPart.ScRuleFactory.CreateRuleCurveFeatureTangent(features1, line1, nullNXOpen_Curve, False, 0.01, 0.5)

textBuilder1.OnFacePlacementProfile.AllowSelfIntersection(True)

Dim rules4(0) As NXOpen.SelectionIntentRule
rules4(0) = curveFeatureTangentRule1
Dim helpPoint2 As NXOpen.Point3d = New NXOpen.Point3d(-56.880335976917863, -6.0840221749458578e-14, 10.000000000000043)
textBuilder1.OnFacePlacementProfile.AddToSection(rules4, line1, nullNXOpen_NXObject, nullNXOpen_NXObject, helpPoint2, NXOpen.Section.Mode.Create, False)

Dim nXObject1 As NXOpen.NXObject = Nothing
nXObject1 = textBuilder1.Commit()

textBuilder1.Destroy()

' -------------------------------------------
' INSERT TEXT 2 AND SEL OFFSET CURVE FOR TEXT
' -------------------------------------------

Dim textBuilder2 As NXOpen.Features.TextBuilder = Nothing
textBuilder2 = workPart.Features.CreateTextBuilder(nullNXOpen_Features_Text)

Dim trimmedAttPartNum As String = attPartnum.Remove( attPartnum.Length - 5 )

textBuilder2.TextString = trimmedAttPartNum
textBuilder2.FrameOnPath.AnchorPosition.Expression.RightHandSide = "50"
textBuilder2.Type = NXOpen.Features.TextBuilder.Types.OnFace
textBuilder2.PlanarFrame.Shear.RightHandSide = "0"
textBuilder2.FrameOnPath.AnchorLocation = NXOpen.GeometricUtilities.FrameOnPathBuilder.AnchorLocationType.Left
textBuilder2.FrameOnPath.AnchorPosition.Expression.RightHandSide = "5"
textBuilder2.FrameOnPath.Height.RightHandSide = "5"
textBuilder2.PrintMarkThickness.RightHandSide = "1"
textBuilder2.FrameOnPath.WScale = 100.0
textBuilder2.FrameOnPath.Offset.RightHandSide = "7"
textBuilder2.SelectFont("Arial", NXOpen.Features.TextBuilder.ScriptOptions.Western)

Dim boundaryFaces2(-1) As NXOpen.Face
Dim faceTangentRule2 As NXOpen.FaceTangentRule = Nothing
faceTangentRule1 = workPart.ScRuleFactory.CreateRuleFaceTangent(pickFace, boundaryFaces2, 0.5)

Dim rules5(0) As NXOpen.SelectionIntentRule
rules5(0) = faceTangentRule1
textBuilder2.PlacementFaces.ReplaceRules(rules5, False)

textBuilder2.OnFacePlacementProfile.SetAllowedEntityTypes(NXOpen.Section.AllowTypes.OnlyCurves)

Dim features2(0) As NXOpen.Features.Feature
features2(0) = aOCS1
Dim line3 As NXOpen.Line = CType(aOCS1.FindObject("CURVE 1"), NXOpen.Line)

Dim curveFeatureTangentRule2 As NXOpen.CurveFeatureTangentRule = Nothing
curveFeatureTangentRule2 = workPart.ScRuleFactory.CreateRuleCurveFeatureTangent(features2, line3, nullNXOpen_Curve, False, 0.01, 0.5)

textBuilder2.OnFacePlacementProfile.AllowSelfIntersection(True)

Dim rules6(0) As NXOpen.SelectionIntentRule
rules6(0) = curveFeatureTangentRule1
Dim helpPoint3 As NXOpen.Point3d = New NXOpen.Point3d(-56.880335976917863, -6.0840221749458578e-14, 10.000000000000043)
textBuilder2.OnFacePlacementProfile.AddToSection(rules6, line3, nullNXOpen_NXObject, nullNXOpen_NXObject, helpPoint3, NXOpen.Section.Mode.Create, False)

Dim nXObject2 As NXOpen.NXObject = Nothing
nXObject2 = textBuilder2.Commit()

textBuilder2.Destroy()

' -------------------------------------------
' INSERT TEXT 3 AND SEL OFFSET CURVE FOR TEXT
' -------------------------------------------

Dim textBuilder3 As NXOpen.Features.TextBuilder = Nothing
textBuilder3 = workPart.Features.CreateTextBuilder(nullNXOpen_Features_Text)

textBuilder3.TextString = attDesc

textBuilder3.FrameOnPath.AnchorPosition.Expression.RightHandSide = "50"
textBuilder3.Type = NXOpen.Features.TextBuilder.Types.OnFace
textBuilder3.PlanarFrame.Shear.RightHandSide = "0"
textBuilder3.FrameOnPath.AnchorLocation = NXOpen.GeometricUtilities.FrameOnPathBuilder.AnchorLocationType.Left
textBuilder3.FrameOnPath.AnchorPosition.Expression.RightHandSide = "5"
textBuilder3.FrameOnPath.Height.RightHandSide = "5"
textBuilder3.PrintMarkThickness.RightHandSide = "1"
textBuilder3.FrameOnPath.WScale = 100.0
textBuilder3.FrameOnPath.Offset.RightHandSide = "14"
textBuilder3.SelectFont("Arial", NXOpen.Features.TextBuilder.ScriptOptions.Western)

Dim boundaryFaces3(-1) As NXOpen.Face
Dim faceTangentRule3 As NXOpen.FaceTangentRule = Nothing
faceTangentRule1 = workPart.ScRuleFactory.CreateRuleFaceTangent(pickFace, boundaryFaces3, 0.5)

Dim rules7(0) As NXOpen.SelectionIntentRule
rules7(0) = faceTangentRule1
textBuilder3.PlacementFaces.ReplaceRules(rules7, False)

textBuilder3.OnFacePlacementProfile.SetAllowedEntityTypes(NXOpen.Section.AllowTypes.OnlyCurves)

Dim features3(0) As NXOpen.Features.Feature
features3(0) = aOCS1
Dim line4 As NXOpen.Line = CType(aOCS1.FindObject("CURVE 1"), NXOpen.Line)

Dim curveFeatureTangentRule3 As NXOpen.CurveFeatureTangentRule = Nothing
curveFeatureTangentRule3 = workPart.ScRuleFactory.CreateRuleCurveFeatureTangent(features3, line4, nullNXOpen_Curve, False, 0.01, 0.5)

textBuilder3.OnFacePlacementProfile.AllowSelfIntersection(True)

Dim rules8(0) As NXOpen.SelectionIntentRule
rules8(0) = curveFeatureTangentRule3
Dim helpPoint4 As NXOpen.Point3d = New NXOpen.Point3d(-56.880335976917863, -6.0840221749458578e-14, 10.000000000000043)
textBuilder3.OnFacePlacementProfile.AddToSection(rules8, line4, nullNXOpen_NXObject, nullNXOpen_NXObject, helpPoint4, NXOpen.Section.Mode.Create, False)

Dim nXObject3 As NXOpen.NXObject = Nothing
nXObject3 = textBuilder3.Commit()

textBuilder3.Destroy()

' ------------------------------
' REVERSE OFFSET CURVE DIRECTION
' ------------------------------
Dim answer As Integer = theUI.NXMessageBox.Show("Offset Curve Direction",
NXOpen.NXMessageBox.DialogType.Question, "Change Offset Curve Direction..?")

If answer = 1 Then

Dim editWithRollbackManager1 As NXOpen.Features.EditWithRollbackManager = Nothing
editWithRollbackManager1 = workPart.Features.StartEditWithRollbackManager(aOCS1, markId1)

Dim aOCSBuilder2 As NXOpen.Features.AOCSBuilder = Nothing
aOCSBuilder2 = workPart.Features.CreateAocsBuilder(aOCS1)

Dim taggedObject2 As NXOpen.TaggedObject = Nothing
taggedObject2 = aOCSBuilder2.Offsets.FindItem(0)

Dim expressionSectionSet2 As NXOpen.ExpressionSectionSet = CType(taggedObject2, NXOpen.ExpressionSectionSet)

section1.ReverseDirectionOfLoop(0)

Dim flipDirection1 As Boolean = Nothing
flipDirection1 = aOCSBuilder2.UpdateSectionData(section1)

Dim feature2 As NXOpen.Features.Feature = Nothing
feature2 = aOCSBuilder2.CommitFeature()

editWithRollbackManager1.UpdateFeature(False)
editWithRollbackManager1.Stop()
editWithRollbackManager1.Destroy()
End If

' ----------------------------------------------
' SELECT TEXT TO EXTRUDE & BODY TO SUBTRACT FROM
' ----------------------------------------------

Dim EdgeOBJ as Edge = pickEdge
Dim text2SubFrom As Body = EdgeOBJ.GetBody()

Dim extrudeBuilder1 As NXOpen.Features.ExtrudeBuilder = Nothing
extrudeBuilder1 = workPart.Features.CreateExtrudeBuilder(nullNXOpen_Features_Feature)

Dim section5 As NXOpen.Section = Nothing
section5 = workPart.Sections.CreateSection(0.0094999999999999998, 0.01, 0.5)

extrudeBuilder1.Section = section5

Dim targetBodies1(0) As NXOpen.Body
Dim nullNXOpen_Body As NXOpen.Body = Nothing
targetBodies1(0) = nullNXOpen_Body

extrudeBuilder1.BooleanOperation.SetTargetBodies(targetBodies1)
extrudeBuilder1.Limits.StartExtend.Value.RightHandSide = "0.5"
extrudeBuilder1.Limits.EndExtend.Value.RightHandSide = "-0.5"
extrudeBuilder1.BooleanOperation.Type = NXOpen.GeometricUtilities.BooleanOperation.BooleanType.Subtract

Dim targetBodies2(0) As NXOpen.Body

targetBodies2(0) = text2SubFrom

extrudeBuilder1.BooleanOperation.SetTargetBodies(targetBodies2)

Dim smartVolumeProfileBuilder1 As NXOpen.GeometricUtilities.SmartVolumeProfileBuilder = Nothing
smartVolumeProfileBuilder1 = extrudeBuilder1.SmartVolumeProfile

Dim features4(0) As NXOpen.Features.Feature
Dim text1 As NXOpen.Features.Text = CType(nXObject1, NXOpen.Features.Text)
features4(0) = text1
Dim features5(0) As NXOpen.Features.Feature
Dim text2 As NXOpen.Features.Text = CType(nXObject2, NXOpen.Features.Text)
features5(0) = text2
Dim features6(0) As NXOpen.Features.Feature
Dim text3 As NXOpen.Features.Text = CType(nXObject3, NXOpen.Features.Text)
features6(0) = text3

Dim curveFeatureRule1 As NXOpen.CurveFeatureRule = Nothing
curveFeatureRule1 = workPart.ScRuleFactory.CreateRuleCurveFeature(features4)
Dim curveFeatureRule2 As NXOpen.CurveFeatureRule = Nothing
curveFeatureRule2 = workPart.ScRuleFactory.CreateRuleCurveFeature(features5)
Dim curveFeatureRule3 As NXOpen.CurveFeatureRule = Nothing
curveFeatureRule3 = workPart.ScRuleFactory.CreateRuleCurveFeature(features6)

Dim rules9(0) As NXOpen.SelectionIntentRule
rules9(0) = curveFeatureRule1
Dim helpPoint5 As NXOpen.Point3d = New NXOpen.Point3d(0.0, 0.0, 0.0)
section5.AddToSection(rules9, nullNXOpen_NXObject, nullNXOpen_NXObject, nullNXOpen_NXObject, helpPoint5, NXOpen.Section.Mode.Create, False)

Dim rules10(0) As NXOpen.SelectionIntentRule
rules10(0) = curveFeatureRule2
Dim helpPoint6 As NXOpen.Point3d = New NXOpen.Point3d(0.0, 0.0, 0.0)
section5.AddToSection(rules10, nullNXOpen_NXObject, nullNXOpen_NXObject, nullNXOpen_NXObject, helpPoint6, NXOpen.Section.Mode.Create, False)

Dim rules11(0) As NXOpen.SelectionIntentRule
rules11(0) = curveFeatureRule3
Dim helpPoint7 As NXOpen.Point3d = New NXOpen.Point3d(0.0, 0.0, 0.0)
section5.AddToSection(rules11, nullNXOpen_NXObject, nullNXOpen_NXObject, nullNXOpen_NXObject, helpPoint7, NXOpen.Section.Mode.Create, False)

Dim origin3 As NXOpen.Point3d = New NXOpen.Point3d(-46.124198330506573, 7.7841263299248453, 10.0)
Dim vector2 As NXOpen.Vector3d = New NXOpen.Vector3d(0.0, 0.0, 1.0)
Dim direction2 As NXOpen.Direction = Nothing
direction2 = workPart.Directions.CreateDirection(origin3, vector2, NXOpen.SmartObject.UpdateOption.WithinModeling)

extrudeBuilder1.Direction = direction2
extrudeBuilder1.ParentFeatureInternal = False

Dim feature3 As NXOpen.Features.Feature = Nothing
feature3 = extrudeBuilder1.CommitFeature()

extrudeBuilder1.Destroy()

'--------------------
'Clear Selection List
'--------------------

Dim partCleanup As NXOpen.PartCleanup = Nothing
partCleanup = theSession.NewPartCleanup()
partCleanup.TurnOffHighlighting = True
partCleanup.DoCleanup()
partCleanup.Dispose()

End Sub

Function SelectAFace(ByVal prompt As String, ByRef selObj As Face) As Selection.Response

Dim theUI As UI = UI.GetUI
Dim title As String = "pickFace"
Dim includeFeatures As Boolean = False
Dim keepHighlighted As Boolean = True
Dim selAction As Selection.SelectionAction = Selection.SelectionAction.ClearAndEnableSpecific
Dim cursor As Point3d
Dim scope As Selection.SelectionScope = Selection.SelectionScope.AnyInAssembly
Dim selectionMask_array(0) As Selection.MaskTriple

With selectionMask_array(0)
.Type = UFConstants.UF_solid_type
.SolidBodySubtype = UFConstants.UF_UI_SEL_FEATURE_ANY_FACE
End With

Dim resp As Selection.Response = theUI.SelectionManager.SelectObject(prompt, _
title, scope, selAction, _
includeFeatures, keepHighlighted, selectionMask_array, _
selObj, cursor)
If resp = Selection.Response.ObjectSelected OrElse resp = Selection.Response.ObjectSelectedByName Then
Return Selection.Response.Ok
Else
Return Selection.Response.Cancel
End If

End Function

Function SelectEdge(ByVal prompt As String, ByRef selObj As TaggedObject) As Selection.Response

Dim theUI As UI = UI.GetUI
Dim title As String = "pickEdge"
Dim includeFeatures As Boolean = False
Dim keepHighlighted As Boolean = True
Dim selAction As Selection.SelectionAction = Selection.SelectionAction.ClearAndEnableSpecific
Dim cursor As Point3d
Dim scope As Selection.SelectionScope = Selection.SelectionScope.WorkPart
Dim selectionMask_array(0) As Selection.MaskTriple

With selectionMask_array(0)
.Type = UFConstants.UF_solid_type
.SolidBodySubtype = UFConstants.UF_UI_SEL_FEATURE_ANY_EDGE
End With

Dim resp As Selection.Response = theUI.SelectionManager.SelectTaggedObject(prompt, _
title, scope, selAction, _
includeFeatures, keepHighlighted, selectionMask_array, _
selobj, cursor)
If resp = Selection.Response.ObjectSelected OrElse resp = Selection.Response.ObjectSelectedByName Then
Return Selection.Response.Ok
Else
Return Selection.Response.Cancel
End If

End Function

Public Function GetUnloadOption(ByVal dummy As String) As Integer

'Unloads the image when the NX session terminates
GetUnloadOption = NXOpen.Session.LibraryUnloadOption.AtTermination

'----Other unload options-------
'Unloads the image immediately after execution within NX
'GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Immediately

'Unloads the image explicitly, via an unload dialog
'GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Explicitly
'-------------------------------

End Function

End Module