-
1
- #1
lj1970
Marine/Ocean
- Nov 26, 2023
- 18
Hello everyone,
I'd like to introduce my latest creation: Captain Hook's Component Creator. Infused with a touch of nautical flair, this tool is designed to streamline the process of component creation within Siemens NX, locally and when integrated with Teamcenter environments.
Under the Hood:
- Local: The tool searches for the first sequential component labeled "-101". It then generates the next available component number. These components aren't saved; they are created for you to save if you are satisfied with the outcome. The journal searches through your library, session, and memory for the component name you have set, checking for available or missing numbers to avoid duplication. The names for the components will be derived from the names of the solid bodies. If a solid body does not have an assigned name, the default name “Panel” will be used.
- Teamcenter: The tool employs a two-round approach to ensure each component is sequentially numbered and accurately tracked in Teamcenter. You can use both the first and second rounds or only the second, depending on your requirements.
Round One: Sets and saves an initial ID number, anchoring the starting point for a sequence.
Round Two: Uses a substitute wildcard number to generate subsequent IDs, which requires experimenting with formats like "*" (star).
Features:
- Smart Sorting: Utilizes EasyWeight or NX's built-in material attributes to sort solid bodies by material name and weight in descending order or retains the order of your initial selection.
- Unit Support: Adapts to both metric (millimeters) and imperial (inches) units within material names.
- EasyWeight Integration: Updates all weight information before component creation with automatic recognition of the unit system.
- Configuration Settings with detailed descriptions at the beginning of the Journal: WaveLink options, flagging created components to avoid duplication, controlling numbering gaps for local environment and Teamcenter option.
This tool is ideal for mechanical engineers and designers using Siemens NX who require an automated method to create components in complex assemblies, particularly beneficial in large-scale projects.
The journal has been thoroughly tested on Siemens NX 2212 and 2306 and is designed for easy customization to fit specific project requirements. For more detailed examples and configuration settings see comments at the beginning of the journal.
Happy designing!
Shared on NXJournaling.com:
Link
and on GitHub:
Link
I'd like to introduce my latest creation: Captain Hook's Component Creator. Infused with a touch of nautical flair, this tool is designed to streamline the process of component creation within Siemens NX, locally and when integrated with Teamcenter environments.
Under the Hood:
- Local: The tool searches for the first sequential component labeled "-101". It then generates the next available component number. These components aren't saved; they are created for you to save if you are satisfied with the outcome. The journal searches through your library, session, and memory for the component name you have set, checking for available or missing numbers to avoid duplication. The names for the components will be derived from the names of the solid bodies. If a solid body does not have an assigned name, the default name “Panel” will be used.
- Teamcenter: The tool employs a two-round approach to ensure each component is sequentially numbered and accurately tracked in Teamcenter. You can use both the first and second rounds or only the second, depending on your requirements.
Round One: Sets and saves an initial ID number, anchoring the starting point for a sequence.
Round Two: Uses a substitute wildcard number to generate subsequent IDs, which requires experimenting with formats like "*" (star).
Features:
- Smart Sorting: Utilizes EasyWeight or NX's built-in material attributes to sort solid bodies by material name and weight in descending order or retains the order of your initial selection.
- Unit Support: Adapts to both metric (millimeters) and imperial (inches) units within material names.
- EasyWeight Integration: Updates all weight information before component creation with automatic recognition of the unit system.
- Configuration Settings with detailed descriptions at the beginning of the Journal: WaveLink options, flagging created components to avoid duplication, controlling numbering gaps for local environment and Teamcenter option.
This tool is ideal for mechanical engineers and designers using Siemens NX who require an automated method to create components in complex assemblies, particularly beneficial in large-scale projects.
The journal has been thoroughly tested on Siemens NX 2212 and 2306 and is designed for easy customization to fit specific project requirements. For more detailed examples and configuration settings see comments at the beginning of the journal.
Happy designing!
Shared on NXJournaling.com:
Link
and on GitHub:
Link
Code:
' Written by Tamas Woller - February 2024, V103
' Journal desciption: Automatically create parts by requesting you a main component name. Select solid bodies to create components for.
' Shared on NXJournaling.com
' Written in VB.Net
' Tested on Siemens NX 2212 and 2306, Native and Teamcenter 13
' V100 - Initial Release - January 2024
' V101 - Body flag system Fix
' V103 - Smart Sorting with EasyWeight or NX's built-in material attributes, Metric (Millimeters) and Imperial (Inches) unit support in Material name, WaveLink Option, Flag Created Components Option, Control Numbering Gaps Option and added Configuration Settings
' V105 - Added notes and minor changes in Output Window
' V107 - Update EasyWeight's EW_Body_Weight attribute before sorting
' V109 - Added 'Maybe' to sorting
' V111 - TC with custom numbering
Imports System
Imports NXOpen
Imports System.Collections.Generic
Imports NXOpen.UF
Imports NXOpen.Assemblies
Imports System.Windows.Forms
Imports System.Text.RegularExpressions
Module NXJournal
Dim theSession As NXOpen.Session = NXOpen.Session.GetSession()
Dim theUFSession As NXOpen.UF.UFSession = NXOpen.UF.UFSession.GetUFSession()
Dim workPart As NXOpen.Part = theSession.Parts.Work
Dim mainAssembly As Part = If(workPart.ComponentAssembly.RootComponent IsNot Nothing, workPart.ComponentAssembly.RootComponent.Prototype, workPart)
Dim unitString As String = "mm"
Dim displayPart As NXOpen.Part = theSession.Parts.Display
Dim theUI As NXOpen.UI = NXOpen.UI.GetUI()
Dim logicalobjects1() As NXOpen.PDM.LogicalObject = Nothing
Dim logicalobjects2() As NXOpen.PDM.LogicalObject = Nothing
Dim sourceobjects1() As NXOpen.NXObject
Dim selectedObjectName As String
Dim mySelectedObjects As New List(Of DisplayableObject)
Dim lw As ListingWindow = theSession.ListingWindow
Dim nXObject2 As NXOpen.NXObject = Nothing
Dim lldirectoryPath As String
Dim materialName As String
Dim bodyWeight As Double
Dim smartsortingfeature As Boolean
Dim assemblyid As String
'------------------------
' Configuration Settings:
' Default Assembly ID name
Dim defaultassemblyid As String = "MyProject-01"
' WaveLink Feature - True or False
Dim wavelinkfeature As Boolean = True
' Smart Sorting - This feature sorts the selected bodies by their material name in descending order. It first considers the initial numerical value found in the material name before the unit (for example, the "12" in "12mm Plywood"). If no numerical value is present, sorting is done alphabetically. Should multiple bodies share the same material, they are then sorted by weight in descending order.
' You'll receive feedback on Material name and weight, so you understand the order presented.
' If it False, it will preserve the order in which you initially clicked on the bodies for selection. - "True", "False" or "Maybe"
Dim smartsortingfeatureQST As String = "Maybe"
' This setting is particularly useful when utilizing the smart sorting feature, as it helps break down material names into segments for efficient sorting and organization. For instance, a material named '12mm Plywood' would be divided at 'mm', allowing the code to sort solids effectively.
' You can adjust settings for "mm" (Millimeter) and "in" (Inch) to whatever you use to describe your materials based on your preferred unit system. Let's say, you are naming your solid bodies like "3/4 Inch Plywood" - then you would change 'ssunitin' to "Inch".
' The journal handles whole or decimal numbers (e.g., "12", "12.5") and fractions specifically for inches (e.g., "1/2"). It automatically adjusts these values by multiplying them by 25.4 to ensure consistency in sorting, allowing you to safely use any of these variants within the same workflow.
Dim ssunitmm As String = "mm"
Dim ssunitin As String = "in"
' Sorting logic use EasyWeight (True) or NX Built-in Material (False) attributes. - True or False
Dim EasyWeightsortinglogic As Boolean = False
' Default Solid Body Name - Assigns a name to any solid body that lacks one, ensuring all bodies are identifiable.
' You can set these names under Reference Sets.
' If you can't see this folder, click on a empty space in Part Navigator / uncheck Timestamp Order OR File / Utilities / Customer Defaults / Gateway / Part Navigator / Display Reference Sets Folder.
Dim defaultsolidbodyname As String = "PANEL"
' Flag Created Components - To prevent duplicating efforts, this option tags processed solid bodies with a 'Component created' attribute. It's an efficient way to track which bodies have already been processed.
' If you want to override this later, simply delete the value of this attribute in Solid body / Properties. - True or False
Dim setcomponentflag As Boolean = False
' Teamcenter Integration Settings - Determines whether the journal operates locally "False" or integrates with Teamcenter. Selecting "Maybe" prompts a question at the start to finalize this setting, tailoring the journal to your specific workflow needs. - "True", "False" or "Maybe".
' If you are using this locally, you will be prompted at the beginning to specify where you want to save your files. If you leave it empty and hit enter, it will use the specified default directory (lldefaultdirectoryPath).
Dim teamcenterIntegrationQST As String = "False"
' Control Numbering Gaps - Only for Local - This feature enables intelligent handling of component numbering. For instance, if you initially create components numbered 101, 102, 103, 104, and 105, but later delete 101 and 103, activating this option will prioritize filling these gaps with new components before proceeding to increment the numbers. It's an efficient method to maintain a continuous sequence and optimize the utilization of available numbers.
' Remember, when removing components, it's important not only to remove them from the assembly but also to close them using File / Close / Selected Parts. This ensures they are removed from memory as well.
' Additionally, if you are working locally and have saved these parts, you should also delete them from the file system to avoid clutter. - True or False
Dim fillTheGap As Boolean = True
' IMPORTANT! Record a Journal first in - Visual Basic (*.vb) - by Developer / Record with Assemblies / New Component. Complete the entire process of creating a new component, then stop the recording. In your saved file, you'll find the following variants (note that prefixes such as 'tc', 'll', and 'wl' won't be included) - the matching words are highlighted:
' partOperationCreateBuilder1.DEFAULTDESTINATIONFOLDER, fileNew1.TEMPLATEFILENAME, fileNew1.UNITS, fileNew1.RELATIONTYPE, fileNew1.TEMPLATEPRESENTATIONNAME and fileNew1.ITEMTYPE.
' Copy paste the values.
'
' Explanation and ID numbering for First and Second Rounds:
' The journal is prepared to follow two different logics in Teamcenter. Let me know if you have a specific case:
' Situation One: Non-specific numbering, following system sequence.
' Goal: Invoke a substitute ID usable in the journal.
' Example: If a new component ID is 160379, try creating another with a substitute ID of 16000* (modify the last digit to "*"). If Teamcenter generates the next available number from 160000, we have found what we were looking for.
' Settings:
' Dim defaultassemblyid As String = "16000*" ' Set our base or default assembly ID.
' Dim assemblyidQST As Boolean = False ' Set to False as the ID follows the previous number without query.
' Dim tcwithtworounds as Boolean = False ' The base - 160000 - is already created, so the first round is unnecessary. Only the second round will use the default ID as a wildcard.
' Dim tcfirstround as String = "" ' Not relevant as the first round is skipped.
' Dim tcsecondround as String = "" ' Should be empty since the default ID is set initially.
' Situation Two: Specific assembly numbers are needed, similar to local logic.
' Goal: Invoke a substitute ID usable in the journal.
' Example: After creating and saving "X184-500-101" as the first component, attempt the next one with "X184-500-10*". If TC automatically generates the next number from 101, it's successful.
' Settings:
' Dim defaultassemblyid As String = "MyProject-01" ' Not relevant here since input is always requested.
' Dim assemblyidQST As Boolean = True ' Set to True to always ask for the base specific assembly ID number on each run. Input example: X184-500.
' Dim tcwithtworounds as Boolean = True ' TC requires a base number to be SAVED first (X184-500-101), allowing it to automatically generate subsequent numbers and create follow-up components in the second. (X184-500-102, etc.).
' Dim tcfirstround as String = "-101" ' This is the number appended to the first round.
' Dim tcsecondround as String = "-10*" ' This is the number appended to the second round.
' TC Settings
Dim tcDefaultDestinationFolder As String = ":NewFolder"
Dim tcTemplateFileName As String = "@DB/GT_mm_template/01"
Dim tcUnits As NXOpen.Part.Units = NXOpen.Part.Units.Millimeters
Dim tcRelationType As String = "master"
Dim tcTemplatePresentationName As String = "Model"
Dim tcItemType As String = "Item"
Dim assemblyidQST As Boolean = False
Dim tcwithtworounds as Boolean = True
Dim tcfirstround as String = "-101"
Dim tcsecondround as String = "-10*"
' Local Settings
Dim llTemplateFileName As String = "model-plain-1-mm-template.prt"
Dim llUnits As NXOpen.Part.Units = NXOpen.Part.Units.Millimeters
Dim llTemplatePresentationName As String = "Model"
Dim lldefaultdirectoryPath As String = "C:\NXPartsFolder\"
Dim llnextAvailableId As Integer = 101
' WaveLink Settings
Dim wlAssociative As Boolean = True
Dim wlFixAtCurrentTimestamp As Boolean = False
Dim wlHideOriginal As Boolean = True
Dim wlInheritDisplayProperties As Boolean = True
Dim wlMakePositionIndependent As Boolean = True
Dim wlCopyThreads As Boolean = True
'------------------------
Sub Main(ByVal args() As String)
lw.Open()
theSession = Session.GetSession()
theUFSession = UFSession.GetUFSession()
workPart = theSession.Parts.Work
displayPart = theSession.Parts.Display
theUI = UI.GetUI()
Dim isFirstSave As Boolean = True
lw.WriteLine("------------------------------------------------------------")
lw.WriteLine("Captain Hook's Component Creator Version: 1.11 NXJ ")
lw.WriteLine(" ")
lw.WriteLine("--------------------------------")
lw.WriteLine("Configuration Settings Overview:")
lw.WriteLine(" ")
lw.WriteLine(" - WaveLink Feature: " & If(wavelinkfeature, "Yes", "No"))
If smartsortingfeatureQST IsNot Nothing AndAlso (smartsortingfeatureQST.Equals("True", StringComparison.OrdinalIgnoreCase) OrElse smartsortingfeatureQST.Equals("False", StringComparison.OrdinalIgnoreCase)) Then
smartsortingfeature = Boolean.Parse(smartsortingfeatureQST)
Else
Dim userResponse As DialogResult = MessageBox.Show("Do you wish to enable Smart Sorting for Components?", "Smart Sorting", MessageBoxButtons.YesNoCancel)
Select Case userResponse
Case DialogResult.Yes
smartsortingfeature = True
Case DialogResult.No
smartsortingfeature = False
Case DialogResult.Cancel
lw.WriteLine(" ")
lw.WriteLine("Abandon ship! We're departing the logbook.")
Return
End Select
End If
lw.WriteLine(" - Smart Sorting: " & If(smartsortingfeature, "Yes", "No"))
If smartsortingfeature Then
If EasyWeightsortinglogic Then
lw.WriteLine(" With EasyWeight attributes")
Else
lw.WriteLine(" With NX Built-in attributes")
End If
Else
lw.WriteLine(" Follow the selection order")
End If
lw.WriteLine(" - Component Created flag: " & If(setcomponentflag, "Yes", "No"))
Dim teamcenterIntegration As Boolean = False
If teamcenterIntegrationQST IsNot Nothing AndAlso (teamcenterIntegrationQST.Equals("True", StringComparison.OrdinalIgnoreCase) OrElse teamcenterIntegrationQST.Equals("False", StringComparison.OrdinalIgnoreCase)) Then
teamcenterIntegration = Boolean.Parse(teamcenterIntegrationQST)
Else
Dim userResponse As DialogResult = MessageBox.Show("Are you working with Teamcenter?", "Teamcenter Integration", MessageBoxButtons.YesNoCancel)
Select Case userResponse
Case DialogResult.Yes
teamcenterIntegration = True
Case DialogResult.No
teamcenterIntegration = False
Case DialogResult.Cancel
lw.WriteLine(" ")
lw.WriteLine("Abandon ship! We're departing the logbook.")
Return
End Select
End If
lw.WriteLine(" - Teamcenter integration: " & If(teamcenterIntegration, "Yes", "No"))
If Not teamcenterIntegration Then
Dim userInput As String = InputBox("Where would you like to save your files? - etc. C:\NXPartsFolder\", "Directory Path")
lldirectoryPath = If(String.IsNullOrWhiteSpace(userInput), lldefaultdirectoryPath, userInput)
If Not lldirectoryPath.EndsWith("\") Then
lldirectoryPath &= "\"
End If
' Check if the directory exists
If Not System.IO.Directory.Exists(lldirectoryPath) Then
Try
System.IO.Directory.CreateDirectory(lldirectoryPath)
lw.WriteLine(" Folder has been created. ")
Catch ex As UnauthorizedAccessException
lw.WriteLine(" ")
lw.WriteLine("Stop the presses! Permission to construct the Folder be refused: " & lldirectoryPath)
lw.WriteLine("Pirate's Proclamation: " & ex.Message)
Return
Catch ex As System.IO.PathTooLongException
lw.WriteLine(" ")
lw.WriteLine("Arr, the map stretches further than the eye can see: " & lldirectoryPath)
lw.WriteLine("Pirate's Proclamation: " & ex.Message)
Return
Catch ex As Exception
lw.WriteLine(" ")
lw.WriteLine("Alas, the winds are not in our favor to form the specified Folder: " & lldirectoryPath)
lw.WriteLine("Pirate's Proclamation: " & ex.Message)
Return
End Try
End If
End If
' Perform the unit check on the main assembly
If mainAssembly.PartUnits = BasePart.Units.Inches Then
unitString = "in"
lw.WriteLine(" - Main Assembly Unit System: Imperial (Inches)")
Else
unitString = "mm"
lw.WriteLine(" - Main Assembly Unit System: Metric (Millimeters)")
End If
If Not teamcenterIntegration Then
lw.WriteLine(" - Save to: " & lldirectoryPath)
lw.WriteLine(" - Fill the gaps in numbers: " & If(fillTheGap, "Yes", "No"))
End If
lw.WriteLine(" - Default Solid Body name: " & defaultsolidbodyname)
If assemblyidQST Then
assemblyid = InputBox("Please enter your required ID Name - etc. MyProject-01", "Component Creator")
If String.IsNullOrEmpty(assemblyid) Then
If Not teamcenterIntegration Then
assemblyid = defaultassemblyid
Else
lw.WriteLine(" ")
lw.WriteLine("Abandon ship! We're departing the logbook.")
Exit Sub
End If
End If
Else
assemblyid = defaultassemblyid
End If
lw.WriteLine(" - Base of AssemblyID: " & assemblyid)
lw.WriteLine("---------------------")
lw.WriteLine(" ")
selectedObjectName = SelectObjects("Hey, select multiple somethings", mySelectedObjects)
Dim markId1 As NXOpen.Session.UndoMarkId
markId1 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Visible, "Component Creator")
Dim nXObject1 As NXOpen.NXObject = Nothing
Dim mySolid As New List(Of Body)
Dim baseAssemblyId As String = assemblyid & "-"
Dim idPart As Integer
Dim usedIds As New SortedSet(Of Integer)()
If Not teamcenterIntegration Then
' Get the IDs from existing files in the directory
For Each file As String In System.IO.Directory.GetFiles(lldirectoryPath, baseAssemblyId & "*")
Dim fileName As String = System.IO.Path.GetFileNameWithoutExtension(file)
If fileName.StartsWith(baseAssemblyId) Then
Dim idString As String = fileName.Substring(baseAssemblyId.Length).TrimStart("-"c)
Dim parts As String() = idString.Split("-"c)
If parts.Length > 0 AndAlso Integer.TryParse(parts(0), idPart) Then
usedIds.Add(idPart)
End If
End If
Next
' Get the IDs from components in the NX session that haven't been saved yet
If workPart.ComponentAssembly.RootComponent IsNot Nothing Then
For Each comp As Component In workPart.ComponentAssembly.RootComponent.GetChildren()
Dim compName As String = comp.DisplayName
If compName.StartsWith(baseAssemblyId) Then
Dim idString As String = compName.Substring(baseAssemblyId.Length).TrimStart("-"c)
Dim parts As String() = idString.Split("-"c)
If parts.Length > 0 AndAlso Integer.TryParse(parts(0), idPart) Then
usedIds.Add(idPart)
End If
End If
Next
End If
' Find the first available ID (filling in the gaps)
If fillTheGap Then
While usedIds.Contains(llnextAvailableId)
llnextAvailableId += 1
End While
Else
' If not filling the gap, find the highest ID and add 1
If usedIds.Count > 0 Then
llnextAvailableId = usedIds.Max + 1
End If
End If
End If
For Each tempComp As DisplayableObject In mySelectedObjects
mySolid.Add(CType(tempComp, Body))
Dim attributePropertiesBuilder1 As NXOpen.AttributePropertiesBuilder = Nothing
Dim createNewComponentBuilder1 As NXOpen.Assemblies.CreateNewComponentBuilder = Nothing
Dim AssemblyidString As String = assemblyid & tcfirstround
Dim body As Body = CType(tempComp, Body)
selectedObjectName = body.Name
If setcomponentflag Then
If IsComponentCreated(body) Then
lw.WriteLine(" ")
lw.WriteLine(" - This solid body already has a component: " & selectedObjectName)
Continue For
End If
End If
If String.IsNullOrEmpty(selectedObjectName) Then
Continue For
End If
If teamcenterIntegration Then
If tcwithtworounds Then
Try
Dim fileNew1 As NXOpen.FileNew = theSession.Parts.FileNew()
Dim partOperationCreateBuilder1 As NXOpen.PDM.PartOperationCreateBuilder = Nothing
partOperationCreateBuilder1 = theSession.PdmSession.CreateCreateOperationBuilder(NXOpen.PDM.PartOperationBuilder.OperationType.Create)
fileNew1.SetPartOperationCreateBuilder(partOperationCreateBuilder1)
partOperationCreateBuilder1.SetOperationSubType(NXOpen.PDM.PartOperationCreateBuilder.OperationSubType.FromTemplate)
partOperationCreateBuilder1.SetModelType("master")
partOperationCreateBuilder1.SetItemType("Item")
partOperationCreateBuilder1.CreateLogicalObjects(logicalobjects1)
sourceobjects1 = logicalobjects1(0).GetUserAttributeSourceObjects()
partOperationCreateBuilder1.DefaultDestinationFolder = tcDefaultDestinationFolder
fileNew1.TemplateFileName = tcTemplateFileName
fileNew1.Units = tcUnits
fileNew1.RelationType = tcRelationType
fileNew1.TemplatePresentationName = tcTemplatePresentationName
fileNew1.ItemType = tcItemType
fileNew1.UseBlankTemplate = False
fileNew1.ApplicationName = "ModelTemplate"
fileNew1.UsesMasterModel = "No"
fileNew1.TemplateType = NXOpen.FileNewTemplateType.Item
fileNew1.Specialization = ""
fileNew1.SetCanCreateAltrep(False)
partOperationCreateBuilder1.SetAddMaster(False)
partOperationCreateBuilder1.CreateLogicalObjects(logicalobjects2)
partOperationCreateBuilder1.SetAddMaster(False)
Dim nullNXOpen_BasePart As NXOpen.BasePart = Nothing
Dim objects1(-1) As NXOpen.NXObject
attributePropertiesBuilder1 = theSession.AttributeManager.CreateAttributePropertiesBuilder(nullNXOpen_BasePart, objects1, NXOpen.AttributePropertiesBuilder.OperationType.Create)
Dim objects2(-1) As NXOpen.NXObject
attributePropertiesBuilder1.SetAttributeObjects(objects2)
Dim objects3(0) As NXOpen.NXObject
objects3(0) = sourceobjects1(0)
attributePropertiesBuilder1.SetAttributeObjects(objects3)
attributePropertiesBuilder1.Title = "DB_PART_NO"
attributePropertiesBuilder1.Category = "Item"
attributePropertiesBuilder1.StringValue = AssemblyidString
attributePropertiesBuilder1.Category = "Item"
Dim changed1 As Boolean = Nothing
changed1 = attributePropertiesBuilder1.CreateAttribute()
Dim attributetitles1(-1) As String
Dim titlepatterns1(-1) As String
nXObject1 = partOperationCreateBuilder1.CreateAttributeTitleToNamingPatternMap(attributetitles1, titlepatterns1)
Dim objects4(0) As NXOpen.NXObject
objects4(0) = logicalobjects1(0)
Dim properties1(0) As NXOpen.NXObject
properties1(0) = nXObject1
Dim errorList1 As NXOpen.ErrorList = Nothing
errorList1 = partOperationCreateBuilder1.AutoAssignAttributesWithNamingPattern(objects4, properties1)
errorList1.Dispose()
attributePropertiesBuilder1.Title = "DB_PART_NAME"
attributePropertiesBuilder1.StringValue = selectedObjectName
attributePropertiesBuilder1.Category = "Item"
Dim changed2 As Boolean = Nothing
changed2 = attributePropertiesBuilder1.CreateAttribute()
fileNew1.MasterFileName = ""
fileNew1.MakeDisplayedPart = False
fileNew1.DisplayPartOption = NXOpen.DisplayPartOption.AllowAdditional
partOperationCreateBuilder1.ValidateLogicalObjectsToCommit()
Dim logicalobjects4(0) As NXOpen.PDM.LogicalObject
logicalobjects4(0) = logicalobjects1(0)
partOperationCreateBuilder1.CreateSpecificationsForLogicalObjects(logicalobjects4)
' Create new component
createNewComponentBuilder1 = workPart.AssemblyManager.CreateNewComponentBuilder()
createNewComponentBuilder1.ReferenceSetName = "MODEL"
createNewComponentBuilder1.ComponentOrigin = NXOpen.Assemblies.CreateNewComponentBuilder.ComponentOriginType.Absolute
createNewComponentBuilder1.OriginalObjectsDeleted = False
createNewComponentBuilder1.ObjectForNewComponent.Clear()
'Non Wavelink add body
If Not wavelinkfeature Then
createNewComponentBuilder1.ObjectForNewComponent.Add(body)
'lw.WriteLine(" Solid body added successfully.")
End If
createNewComponentBuilder1.NewFile = fileNew1
Dim nXObject2 As NXOpen.NXObject = Nothing
nXObject2 = createNewComponentBuilder1.Commit()
lw.WriteLine("")
lw.WriteLine(" - First component for: " & selectedObjectName & " created.")
Dim bodyToAdd As NXOpen.Body = CType(body, NXOpen.Body)
If smartsortingfeature Then
If EasyWeightsortinglogic Then
Try
materialName = bodyToAdd.GetStringAttribute("EW_Material")
Catch exInner As Exception
materialName = "Not specified"
End Try
Try
bodyWeight = bodyToAdd.GetRealAttribute("EW_Body_Weight")
Catch exInner As Exception
bodyWeight = -1
End Try
Else
Try
materialName = GetMaterialName(bodyToAdd)
Catch exInner As Exception
materialName = "Not specified"
End Try
Try
bodyWeight = GetBodyWeight(bodyToAdd)
Catch exInner As Exception
bodyWeight = -1
End Try
End If
lw.WriteLine(String.Format(" Material Name: {0}", materialName))
lw.WriteLine(String.Format(" Weight: {0}", bodyWeight.ToString()))
End If
Dim newComponent As NXOpen.Assemblies.Component = TryCast(nXObject2, NXOpen.Assemblies.Component)
Dim newComponentPart As Part = CType(newComponent.Prototype, Part)
If wavelinkfeature Then
' Change the work part to the new component's part
theSession.Parts.SetWork(newComponentPart)
' Setup the WaveLinkBuilder in the new component's context
Dim waveLinkBuilder As Features.WaveLinkBuilder = newComponentPart.BaseFeatures.CreateWaveLinkBuilder(Nothing)
waveLinkBuilder.Type = Features.WaveLinkBuilder.Types.BodyLink
waveLinkBuilder.CopyThreads = False
Dim extractFaceBuilder As Features.ExtractFaceBuilder = waveLinkBuilder.ExtractFaceBuilder
extractFaceBuilder.FaceOption = Features.ExtractFaceBuilder.FaceOptionType.FaceChain
extractFaceBuilder.ParentPart = Features.ExtractFaceBuilder.ParentPartType.OtherPart
extractFaceBuilder.Associative = wlAssociative
extractFaceBuilder.FixAtCurrentTimestamp = wlFixAtCurrentTimestamp
extractFaceBuilder.HideOriginal = wlHideOriginal
extractFaceBuilder.InheritDisplayProperties = wlInheritDisplayProperties
extractFaceBuilder.MakePositionIndependent = wlMakePositionIndependent
extractFaceBuilder.CopyThreads = wlCopyThreads
Dim selectObjectList As SelectObjectList = extractFaceBuilder.BodyToExtract
selectObjectList.Add(body)
waveLinkBuilder.Commit()
lw.WriteLine(" WaveLink added successfully.")
waveLinkBuilder.Destroy()
End If
' Mark the original body as processed
If setcomponentflag Then
SetComponentCreated(body, True)
End If
theSession.Parts.SetWork(workPart)
If isFirstSave Then
Dim partSaveStatus As NXOpen.PartSaveStatus = Nothing
Dim newPart As NXOpen.Part = CType(newComponent.Prototype, NXOpen.Part)
Try
partSaveStatus = newPart.Save(NXOpen.BasePart.SaveComponents.False, NXOpen.BasePart.CloseAfterSave.False)
Catch ex As NXOpen.NXException
Catch ex As Exception
End Try
If partSaveStatus IsNot Nothing Then
partSaveStatus.Dispose()
End If
lw.WriteLine(" Saved to Teamcenter: " & AssemblyidString)
'lw.WriteLine(" ")
'lw.WriteLine("A friendly nudge: the remaining components are still drifting in the digital")
'lw.WriteLine("ether, unsaved. Do cast an eye, delete, if the stars are out of alignment,")
'lw.WriteLine("and proceed as the universe dictates.")
isFirstSave = False
Else
End If
Catch ex As Exception When ex.Message.Contains("The new filename is not a valid file specification")
Dim markId2 As NXOpen.Session.UndoMarkId
markId2 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Visible, "Component Creator")
AssemblyidString = assemblyid & tcsecondround
Dim fileNew1 As NXOpen.FileNew = theSession.Parts.FileNew()
Dim partOperationCreateBuilder1 As NXOpen.PDM.PartOperationCreateBuilder = Nothing
partOperationCreateBuilder1 = theSession.PdmSession.CreateCreateOperationBuilder(NXOpen.PDM.PartOperationBuilder.OperationType.Create)
fileNew1.SetPartOperationCreateBuilder(partOperationCreateBuilder1)
partOperationCreateBuilder1.SetOperationSubType(NXOpen.PDM.PartOperationCreateBuilder.OperationSubType.FromTemplate)
partOperationCreateBuilder1.SetModelType("master")
partOperationCreateBuilder1.SetItemType("Item")
partOperationCreateBuilder1.CreateLogicalObjects(logicalobjects1)
sourceobjects1 = logicalobjects1(0).GetUserAttributeSourceObjects()
partOperationCreateBuilder1.DefaultDestinationFolder = tcDefaultDestinationFolder
fileNew1.TemplateFileName = tcTemplateFileName
fileNew1.Units = tcUnits
fileNew1.RelationType = tcRelationType
fileNew1.TemplatePresentationName = tcTemplatePresentationName
fileNew1.ItemType = tcItemType
fileNew1.UseBlankTemplate = False
fileNew1.ApplicationName = "ModelTemplate"
fileNew1.UsesMasterModel = "No"
fileNew1.TemplateType = NXOpen.FileNewTemplateType.Item
fileNew1.Specialization = ""
fileNew1.SetCanCreateAltrep(False)
partOperationCreateBuilder1.SetAddMaster(False)
partOperationCreateBuilder1.CreateLogicalObjects(logicalobjects2)
partOperationCreateBuilder1.SetAddMaster(False)
Dim nullNXOpen_BasePart As NXOpen.BasePart = Nothing
Dim objects1(-1) As NXOpen.NXObject
attributePropertiesBuilder1 = theSession.AttributeManager.CreateAttributePropertiesBuilder(nullNXOpen_BasePart, objects1, NXOpen.AttributePropertiesBuilder.OperationType.Create)
Dim objects2(-1) As NXOpen.NXObject
attributePropertiesBuilder1.SetAttributeObjects(objects2)
Dim objects3(0) As NXOpen.NXObject
objects3(0) = sourceobjects1(0)
attributePropertiesBuilder1.SetAttributeObjects(objects3)
attributePropertiesBuilder1.Title = "DB_PART_NO"
attributePropertiesBuilder1.Category = "Item"
attributePropertiesBuilder1.StringValue = AssemblyidString
attributePropertiesBuilder1.Category = "Item"
Dim changed1 As Boolean = Nothing
changed1 = attributePropertiesBuilder1.CreateAttribute()
Dim attributetitles1(-1) As String
Dim titlepatterns1(-1) As String
nXObject1 = partOperationCreateBuilder1.CreateAttributeTitleToNamingPatternMap(attributetitles1, titlepatterns1)
Dim objects4(0) As NXOpen.NXObject
objects4(0) = logicalobjects1(0)
Dim properties1(0) As NXOpen.NXObject
properties1(0) = nXObject1
Dim errorList1 As NXOpen.ErrorList = Nothing
errorList1 = partOperationCreateBuilder1.AutoAssignAttributesWithNamingPattern(objects4, properties1)
errorList1.Dispose()
attributePropertiesBuilder1.Title = "DB_PART_NAME"
attributePropertiesBuilder1.StringValue = selectedObjectName
attributePropertiesBuilder1.Category = "Item"
Dim changed2 As Boolean = Nothing
changed2 = attributePropertiesBuilder1.CreateAttribute()
fileNew1.MasterFileName = ""
fileNew1.MakeDisplayedPart = False
fileNew1.DisplayPartOption = NXOpen.DisplayPartOption.AllowAdditional
partOperationCreateBuilder1.ValidateLogicalObjectsToCommit()
Dim logicalobjects4(0) As NXOpen.PDM.LogicalObject
logicalobjects4(0) = logicalobjects1(0)
partOperationCreateBuilder1.CreateSpecificationsForLogicalObjects(logicalobjects4)
createNewComponentBuilder1 = workPart.AssemblyManager.CreateNewComponentBuilder()
createNewComponentBuilder1.ReferenceSetName = "MODEL"
createNewComponentBuilder1.ComponentOrigin = NXOpen.Assemblies.CreateNewComponentBuilder.ComponentOriginType.Absolute
createNewComponentBuilder1.OriginalObjectsDeleted = False
createNewComponentBuilder1.ObjectForNewComponent.Clear()
'Non Wavelink add body
If Not wavelinkfeature Then
createNewComponentBuilder1.ObjectForNewComponent.Add(body)
'lw.WriteLine(" Solid body added successfully.")
End If
createNewComponentBuilder1.NewFile = fileNew1
Dim nXObject2 As NXOpen.NXObject = Nothing
nXObject2 = createNewComponentBuilder1.Commit()
lw.WriteLine(" ")
lw.WriteLine(" - Component created for: " & selectedObjectName)
Dim bodyToAdd As NXOpen.Body = CType(body, NXOpen.Body)
If smartsortingfeature Then
If EasyWeightsortinglogic Then
Try
materialName = bodyToAdd.GetStringAttribute("EW_Material")
Catch exInner As Exception
materialName = "Not specified"
End Try
Try
bodyWeight = bodyToAdd.GetRealAttribute("EW_Body_Weight")
Catch exInner As Exception
bodyWeight = -1
End Try
Else
Try
materialName = GetMaterialName(bodyToAdd)
Catch exInner As Exception
materialName = "Not specified"
End Try
Try
bodyWeight = GetBodyWeight(bodyToAdd)
Catch exInner As Exception
bodyWeight = -1
End Try
End If
lw.WriteLine(String.Format(" Material Name: {0}", materialName))
lw.WriteLine(String.Format(" Weight: {0}", bodyWeight.ToString()))
End If
Dim newComponent As NXOpen.Assemblies.Component = TryCast(nXObject2, NXOpen.Assemblies.Component)
Dim newComponentPart As Part = CType(newComponent.Prototype, Part)
If wavelinkfeature Then
' Change the work part to the new component's part
theSession.Parts.SetWork(newComponentPart)
' Setup the WaveLinkBuilder in the new component's context
Dim waveLinkBuilder As Features.WaveLinkBuilder = newComponentPart.BaseFeatures.CreateWaveLinkBuilder(Nothing)
waveLinkBuilder.Type = Features.WaveLinkBuilder.Types.BodyLink
Dim extractFaceBuilder As Features.ExtractFaceBuilder = waveLinkBuilder.ExtractFaceBuilder
extractFaceBuilder.FaceOption = Features.ExtractFaceBuilder.FaceOptionType.FaceChain
extractFaceBuilder.ParentPart = Features.ExtractFaceBuilder.ParentPartType.OtherPart
extractFaceBuilder.Associative = wlAssociative
extractFaceBuilder.FixAtCurrentTimestamp = wlFixAtCurrentTimestamp
extractFaceBuilder.HideOriginal = wlHideOriginal
extractFaceBuilder.InheritDisplayProperties = wlInheritDisplayProperties
extractFaceBuilder.MakePositionIndependent = wlMakePositionIndependent
extractFaceBuilder.CopyThreads = wlCopyThreads
Dim selectObjectList As SelectObjectList = extractFaceBuilder.BodyToExtract
selectObjectList.Add(body)
waveLinkBuilder.Commit()
lw.WriteLine(" WaveLink added successfully.")
waveLinkBuilder.Destroy()
End If
If setcomponentflag Then
SetComponentCreated(body, True)
End If
theSession.Parts.SetWork(workPart)
Catch ex As Exception
lw.WriteLine(" ")
lw.WriteLine("Yo ho, mates, we've hit a snag... an error has marooned us: " & ex.Message)
lw.WriteLine("Pirate's Proclamation: " & ex.StackTrace)
Finally
If createNewComponentBuilder1 IsNot Nothing Then
createNewComponentBuilder1.Destroy()
End If
If attributePropertiesBuilder1 IsNot Nothing Then
attributePropertiesBuilder1.Destroy()
End If
End Try
Else
Try
Dim markId2 As NXOpen.Session.UndoMarkId
markId2 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Visible, "Component Creator")
AssemblyidString = assemblyid & tcsecondround
Dim fileNew1 As NXOpen.FileNew = theSession.Parts.FileNew()
Dim partOperationCreateBuilder1 As NXOpen.PDM.PartOperationCreateBuilder = Nothing
partOperationCreateBuilder1 = theSession.PdmSession.CreateCreateOperationBuilder(NXOpen.PDM.PartOperationBuilder.OperationType.Create)
fileNew1.SetPartOperationCreateBuilder(partOperationCreateBuilder1)
partOperationCreateBuilder1.SetOperationSubType(NXOpen.PDM.PartOperationCreateBuilder.OperationSubType.FromTemplate)
partOperationCreateBuilder1.SetModelType("master")
partOperationCreateBuilder1.SetItemType("Item")
partOperationCreateBuilder1.CreateLogicalObjects(logicalobjects1)
sourceobjects1 = logicalobjects1(0).GetUserAttributeSourceObjects()
partOperationCreateBuilder1.DefaultDestinationFolder = tcDefaultDestinationFolder
fileNew1.TemplateFileName = tcTemplateFileName
fileNew1.Units = tcUnits
fileNew1.RelationType = tcRelationType
fileNew1.TemplatePresentationName = tcTemplatePresentationName
fileNew1.ItemType = tcItemType
fileNew1.UseBlankTemplate = False
fileNew1.ApplicationName = "ModelTemplate"
fileNew1.UsesMasterModel = "No"
fileNew1.TemplateType = NXOpen.FileNewTemplateType.Item
fileNew1.Specialization = ""
fileNew1.SetCanCreateAltrep(False)
partOperationCreateBuilder1.SetAddMaster(False)
partOperationCreateBuilder1.CreateLogicalObjects(logicalobjects2)
partOperationCreateBuilder1.SetAddMaster(False)
Dim nullNXOpen_BasePart As NXOpen.BasePart = Nothing
Dim objects1(-1) As NXOpen.NXObject
attributePropertiesBuilder1 = theSession.AttributeManager.CreateAttributePropertiesBuilder(nullNXOpen_BasePart, objects1, NXOpen.AttributePropertiesBuilder.OperationType.Create)
Dim objects2(-1) As NXOpen.NXObject
attributePropertiesBuilder1.SetAttributeObjects(objects2)
Dim objects3(0) As NXOpen.NXObject
objects3(0) = sourceobjects1(0)
attributePropertiesBuilder1.SetAttributeObjects(objects3)
attributePropertiesBuilder1.Title = "DB_PART_NO"
attributePropertiesBuilder1.Category = "Item"
attributePropertiesBuilder1.StringValue = AssemblyidString
attributePropertiesBuilder1.Category = "Item"
Dim changed1 As Boolean = Nothing
changed1 = attributePropertiesBuilder1.CreateAttribute()
Dim attributetitles1(-1) As String
Dim titlepatterns1(-1) As String
nXObject1 = partOperationCreateBuilder1.CreateAttributeTitleToNamingPatternMap(attributetitles1, titlepatterns1)
Dim objects4(0) As NXOpen.NXObject
objects4(0) = logicalobjects1(0)
Dim properties1(0) As NXOpen.NXObject
properties1(0) = nXObject1
Dim errorList1 As NXOpen.ErrorList = Nothing
errorList1 = partOperationCreateBuilder1.AutoAssignAttributesWithNamingPattern(objects4, properties1)
errorList1.Dispose()
attributePropertiesBuilder1.Title = "DB_PART_NAME"
attributePropertiesBuilder1.StringValue = selectedObjectName
attributePropertiesBuilder1.Category = "Item"
Dim changed2 As Boolean = Nothing
changed2 = attributePropertiesBuilder1.CreateAttribute()
fileNew1.MasterFileName = ""
fileNew1.MakeDisplayedPart = False
fileNew1.DisplayPartOption = NXOpen.DisplayPartOption.AllowAdditional
partOperationCreateBuilder1.ValidateLogicalObjectsToCommit()
Dim logicalobjects4(0) As NXOpen.PDM.LogicalObject
logicalobjects4(0) = logicalobjects1(0)
partOperationCreateBuilder1.CreateSpecificationsForLogicalObjects(logicalobjects4)
createNewComponentBuilder1 = workPart.AssemblyManager.CreateNewComponentBuilder()
createNewComponentBuilder1.ReferenceSetName = "MODEL"
createNewComponentBuilder1.ComponentOrigin = NXOpen.Assemblies.CreateNewComponentBuilder.ComponentOriginType.Absolute
createNewComponentBuilder1.OriginalObjectsDeleted = False
createNewComponentBuilder1.ObjectForNewComponent.Clear()
'Non Wavelink add body
If Not wavelinkfeature Then
createNewComponentBuilder1.ObjectForNewComponent.Add(body)
'lw.WriteLine(" Solid body added successfully.")
End If
createNewComponentBuilder1.NewFile = fileNew1
Dim nXObject2 As NXOpen.NXObject = Nothing
nXObject2 = createNewComponentBuilder1.Commit()
lw.WriteLine(" ")
lw.WriteLine(" - Component created for: " & selectedObjectName)
Dim bodyToAdd As NXOpen.Body = CType(body, NXOpen.Body)
If smartsortingfeature Then
If EasyWeightsortinglogic Then
Try
materialName = bodyToAdd.GetStringAttribute("EW_Material")
Catch exInner As Exception
materialName = "Not specified"
End Try
Try
bodyWeight = bodyToAdd.GetRealAttribute("EW_Body_Weight")
Catch exInner As Exception
bodyWeight = -1
End Try
Else
Try
materialName = GetMaterialName(bodyToAdd)
Catch exInner As Exception
materialName = "Not specified"
End Try
Try
bodyWeight = GetBodyWeight(bodyToAdd)
Catch exInner As Exception
bodyWeight = -1
End Try
End If
lw.WriteLine(String.Format(" Material Name: {0}", materialName))
lw.WriteLine(String.Format(" Weight: {0}", bodyWeight.ToString()))
End If
Dim newComponent As NXOpen.Assemblies.Component = TryCast(nXObject2, NXOpen.Assemblies.Component)
Dim newComponentPart As Part = CType(newComponent.Prototype, Part)
If wavelinkfeature Then
' Change the work part to the new component's part
theSession.Parts.SetWork(newComponentPart)
' Setup the WaveLinkBuilder in the new component's context
Dim waveLinkBuilder As Features.WaveLinkBuilder = newComponentPart.BaseFeatures.CreateWaveLinkBuilder(Nothing)
waveLinkBuilder.Type = Features.WaveLinkBuilder.Types.BodyLink
Dim extractFaceBuilder As Features.ExtractFaceBuilder = waveLinkBuilder.ExtractFaceBuilder
extractFaceBuilder.FaceOption = Features.ExtractFaceBuilder.FaceOptionType.FaceChain
extractFaceBuilder.ParentPart = Features.ExtractFaceBuilder.ParentPartType.OtherPart
extractFaceBuilder.Associative = wlAssociative
extractFaceBuilder.FixAtCurrentTimestamp = wlFixAtCurrentTimestamp
extractFaceBuilder.HideOriginal = wlHideOriginal
extractFaceBuilder.InheritDisplayProperties = wlInheritDisplayProperties
extractFaceBuilder.MakePositionIndependent = wlMakePositionIndependent
extractFaceBuilder.CopyThreads = wlCopyThreads
Dim selectObjectList As SelectObjectList = extractFaceBuilder.BodyToExtract
selectObjectList.Add(body)
waveLinkBuilder.Commit()
lw.WriteLine(" WaveLink added successfully.")
waveLinkBuilder.Destroy()
End If
' Mark the original body as processed
If setcomponentflag Then
SetComponentCreated(body, True)
End If
theSession.Parts.SetWork(workPart)
Catch ex As Exception
lw.WriteLine(" ")
lw.WriteLine("Yo ho, mates, we've hit a snag... an error has marooned us: " & ex.Message)
lw.WriteLine("Pirate's Proclamation: " & ex.StackTrace)
Finally
If createNewComponentBuilder1 IsNot Nothing Then
createNewComponentBuilder1.Destroy()
End If
If attributePropertiesBuilder1 IsNot Nothing Then
attributePropertiesBuilder1.Destroy()
End If
End Try
End If
Else
' Setup for local (non-Teamcenter) environment
Try
Dim markId2 As NXOpen.Session.UndoMarkId
markId2 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Visible, "Component Creator")
Dim fileNew1 As NXOpen.FileNew = theSession.Parts.FileNew()
' Construct the new file name with the next available ID
Dim newFileName As String = lldirectoryPath & baseAssemblyId & llnextAvailableId.ToString("D3") & "-" & selectedObjectName & ".prt"
Dim simpleFileName As String = baseAssemblyId & llnextAvailableId.ToString("D3") & "-" & selectedObjectName & ".prt"
fileNew1.NewFileName = newFileName
fileNew1.UseBlankTemplate = False
fileNew1.ApplicationName = "ModelTemplate"
fileNew1.Units = llUnits
fileNew1.TemplateType = NXOpen.FileNewTemplateType.Item
fileNew1.TemplatePresentationName = llTemplatePresentationName
fileNew1.AllowTemplatePostPartCreationAction(False)
fileNew1.TemplateFileName = llTemplateFileName
fileNew1.MakeDisplayedPart = False
createNewComponentBuilder1 = workPart.AssemblyManager.CreateNewComponentBuilder()
createNewComponentBuilder1.DefiningObjectsAdded = False
createNewComponentBuilder1.NewComponentName = selectedObjectName.ToString
createNewComponentBuilder1.ReferenceSetName = "MODEL"
createNewComponentBuilder1.OriginalObjectsDeleted = False
createNewComponentBuilder1.DefiningObjectsAdded = True
createNewComponentBuilder1.ComponentOrigin = NXOpen.Assemblies.CreateNewComponentBuilder.ComponentOriginType.Absolute
createNewComponentBuilder1.ObjectForNewComponent.Clear()
createNewComponentBuilder1.NewFile = fileNew1
Dim bodyToAdd As NXOpen.Body = CType(tempComp, NXOpen.Body)
lw.WriteLine(" ")
lw.WriteLine(String.Format(" - Processing Body: " & selectedObjectName))
If smartsortingfeature Then
If EasyWeightsortinglogic Then
Try
materialName = bodyToAdd.GetStringAttribute("EW_Material")
Catch exInner As Exception
materialName = "Not specified"
End Try
Try
bodyWeight = bodyToAdd.GetRealAttribute("EW_Body_Weight")
Catch exInner As Exception
bodyWeight = -1 ' Use -1 or another indicative value to signify that the attribute was not found
End Try
Else
Try
materialName = GetMaterialName(bodyToAdd)
Catch exInner As Exception
materialName = "Not specified"
End Try
Try
bodyWeight = GetBodyWeight(bodyToAdd)
Catch exInner As Exception
bodyWeight = -1 ' Use -1 or another indicative value to signify that the attribute was not found
End Try
End If
lw.WriteLine(String.Format(" Material Name: {0}", materialName))
lw.WriteLine(String.Format(" Weight: {0}", bodyWeight.ToString()))
End If
' Add a selected solid body to the component without Wavelink
If Not wavelinkfeature Then
Dim added1 As Boolean = createNewComponentBuilder1.ObjectForNewComponent.Add(bodyToAdd)
lw.WriteLine(" Solid body added successfully.")
End If
nXObject1 = createNewComponentBuilder1.Commit()
lw.WriteLine(" Component created as: " & simpleFileName)
If wavelinkfeature Then
Dim newComponent As NXOpen.Assemblies.Component = CType(nXObject1, NXOpen.Assemblies.Component)
Dim newComponentPart As NXOpen.Part = CType(newComponent.Prototype, NXOpen.Part)
' Switch to the new component part to work within its context
Dim partLoadStatus As NXOpen.PartLoadStatus = Nothing
theSession.Parts.SetWorkComponent(newComponent, NXOpen.PartCollection.RefsetOption.Current, NXOpen.PartCollection.WorkComponentOption.Visible, partLoadStatus)
If partLoadStatus IsNot Nothing Then partLoadStatus.Dispose()
' Setup the WaveLinkBuilder in the new component's context
Dim waveLinkBuilder As Features.WaveLinkBuilder = newComponentPart.BaseFeatures.CreateWaveLinkBuilder(Nothing)
waveLinkBuilder.Type = Features.WaveLinkBuilder.Types.BodyLink
Dim extractFaceBuilder As Features.ExtractFaceBuilder = waveLinkBuilder.ExtractFaceBuilder
extractFaceBuilder.FaceOption = Features.ExtractFaceBuilder.FaceOptionType.FaceChain
extractFaceBuilder.ParentPart = Features.ExtractFaceBuilder.ParentPartType.OtherPart
extractFaceBuilder.Associative = wlAssociative
extractFaceBuilder.FixAtCurrentTimestamp = wlFixAtCurrentTimestamp
extractFaceBuilder.HideOriginal = wlHideOriginal
extractFaceBuilder.InheritDisplayProperties = wlInheritDisplayProperties
extractFaceBuilder.MakePositionIndependent = wlMakePositionIndependent
extractFaceBuilder.CopyThreads = wlCopyThreads
Dim selectObjectList As SelectObjectList = extractFaceBuilder.BodyToExtract
' Setting up ScCollector and SelectionIntentRule for the body
Dim scCollector As NXOpen.ScCollector = extractFaceBuilder.ExtractBodyCollector
Dim selectionIntentRuleOptions As NXOpen.SelectionIntentRuleOptions = newComponentPart.ScRuleFactory.CreateRuleOptions()
selectionIntentRuleOptions.SetSelectedFromInactive(False)
Dim bodies() As Body = {bodyToAdd}
Dim bodyDumbRule As NXOpen.BodyDumbRule = newComponentPart.ScRuleFactory.CreateRuleBodyDumb(bodies, True, selectionIntentRuleOptions)
selectionIntentRuleOptions.Dispose()
Dim rules() As NXOpen.SelectionIntentRule = {bodyDumbRule}
scCollector.ReplaceRules(rules, False)
waveLinkBuilder.Commit()
lw.WriteLine(" WaveLink added successfully.")
waveLinkBuilder.Destroy()
End If
' Mark the original body as processed
If setcomponentflag Then
SetComponentCreated(body, True)
End If
createNewComponentBuilder1.Destroy()
theSession.CleanUpFacetedFacesAndEdges()
theSession.Parts.SetWork(workPart)
' Add the new ID to the set to track it within the session
usedIds.Add(llnextAvailableId)
' Find the next available ID based on the fillTheGap setting
If fillTheGap Then
llnextAvailableId += 1
While usedIds.Contains(llnextAvailableId)
llnextAvailableId += 1
End While
Else
llnextAvailableId = usedIds.Max + 1
End If
Catch ex As NXOpen.NXException When ex.Message.Contains("File already exists")
lw.WriteLine(" ")
lw.WriteLine("We attempted to fill the gap during component creation, but")
lw.WriteLine("encountered an error because one or more removed parts are still")
lw.WriteLine("in memory. Please close them in the NX session as well.")
lw.WriteLine("Go to File > Close > Selected Parts.")
Catch ex As Exception
lw.WriteLine("By Blackbeard's ghost, we're in uncharted waters... a complication has arisen: " & ex.Message)
Finally
End Try
End If
Next
lw.WriteLine(" ")
Dim endQuotes As New List(Of String) From {
"Our expedition into the dusk reaches its twilight. Now, who recalls the spot of our anchorage?",
"Our odyssey across the realms of power concludes.",
"Our dance with destiny ends in silence.",
"Our voyage through the storm finds its harbor in the void.",
"Our voyage has sailed into the sunset. Now, who remembers where we parked?",
"We've run out of road. Next stop: uncharted couch territories.",
"That's a wrap on our adventure. Please exit through the gift shop.",
"The end of our quest is here. Time to hang up our capes.",
"We've navigated the void and returned. Yet, the darkness lingers, an eternal companion.",
"Our expedition's final log. Beam us up, there's no intelligent life down here!",
"Our shared path diverges here. May your socks always match in future adventures.",
"The torch of our adventure dims, its light flickering one final moment."
}
Dim rnd As New Random()
Dim index As Integer = rnd.Next(endQuotes.Count)
Dim selectedQuote As String = endQuotes(index)
lw.WriteLine(selectedQuote)
lw.WriteLine(" ")
'lw.WriteLine("----------")
End Sub
Function IsComponentCreated(ByVal body As Body) As Boolean
Try
Dim attrValue As String = ""
' Determine the target body based on whether it's an occurrence
Dim targetBody As Body = If(body.IsOccurrence, body.Prototype, body)
' Check if the attribute exists and retrieve its value
If targetBody.HasUserAttribute("Component_created", NXObject.AttributeType.String, -1) Then
attrValue = targetBody.GetStringAttribute("Component_created")
End If
' If the attribute exists but is empty, interpret it as "no" (False)
If String.IsNullOrEmpty(attrValue) Then
Return False
End If
' If the attribute value is a valid boolean string, return its boolean equivalent
If attrValue.Equals("True", StringComparison.OrdinalIgnoreCase) OrElse
attrValue.Equals("False", StringComparison.OrdinalIgnoreCase) Then
Return Boolean.Parse(attrValue)
Else
' If the attribute value is not a recognized boolean string, log a message and interpret as False
lw.WriteLine("Arr, this 'Component_created' be flying a foreign flag: '" & attrValue & "' for " & If(body.IsOccurrence, "instance: ", "body: ") & targetBody.JournalIdentifier)
Return False
End If
Catch ex As NXOpen.NXException
lw.WriteLine("Shiver me timbers, we've sailed into a storm... a mistake has been spotted: " & ex.Message)
End Try
' Return false if attribute not found, not valid, or any exception occurs
Return False
End Function
Sub SetComponentCreated(ByVal body As Body, ByVal created As Boolean)
Try
Dim targetBody As Body = body
' If the body is an occurrence, use the prototype body for setting attributes
If body.IsOccurrence Then
targetBody = body.Prototype
End If
' Set the user attribute on the target body
targetBody.SetUserAttribute("Component_created", -1, created.ToString(), Update.Option.Now)
' Log a success message indicating the attribute was set
'lw.WriteLine("Attribute 'Component_created' set to " & created.ToString() & " for " & If(body.IsOccurrence, "instance: ", "body: ") & targetBody.JournalIdentifier)
Catch ex As NXOpen.NXException
lw.WriteLine("Hitch in casting the line 'Component_created' on " & If(body.IsOccurrence, "instance: ", "body: ") & body.JournalIdentifier & " - " & ex.Message)
End Try
End Sub
Function SelectObjects(prompt As String, ByRef dispObj As List(Of DisplayableObject)) As Boolean
Dim selObj As NXObject()
Dim title As String = "Select solid bodies"
Dim includeFeatures As Boolean = False
Dim keepHighlighted As Boolean = False
Dim selAction As Selection.SelectionAction = Selection.SelectionAction.ClearAndEnableSpecific
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_SOLID_BODY
End With
Dim resp As Selection.Response = theUI.SelectionManager.SelectObjects(prompt,
title, scope, selAction,
includeFeatures, keepHighlighted, selectionMask_array,
selObj)
If resp = Selection.Response.ObjectSelected OrElse
resp = Selection.Response.ObjectSelectedByName OrElse
resp = Selection.Response.Ok Then
If selObj IsNot Nothing AndAlso selObj.Length > 0 Then
For Each item As NXObject In selObj
If String.IsNullOrEmpty(item.Name) Then
item.SetName(defaultsolidbodyname)
End If
dispObj.Add(CType(item, DisplayableObject))
Next
' Update EW_Body_Weight if EasyWeightsortinglogic is true
If EasyWeightsortinglogic Then
For Each body As DisplayableObject In dispObj
If TypeOf body Is Body Then
UpdateBodyWeight(CType(body, Body))
End If
Next
lw.WriteLine("")
lw.WriteLine(" - Successfully updated the Weight information.")
lw.WriteLine("")
End If
' SmartSort objects
If smartsortingfeature Then
If EasyWeightsortinglogic Then
Try
dispObj.Sort(Function(a, b)
Dim aMat As String = Nothing
Dim bMat As String = Nothing
Dim aWeight As Double = 0
Dim bWeight As Double = 0
Dim primaryResult As Integer = 0
Try
aMat = a.GetStringAttribute("EW_Material")
Catch ex As Exception
aMat = "zzzzz"
End Try
Try
bMat = b.GetStringAttribute("EW_Material")
Catch ex As Exception
bMat = "zzzzz"
End Try
Try
aWeight = a.GetRealAttribute("EW_Body_Weight")
Catch ex As Exception
aWeight = 0
End Try
Try
bWeight = b.GetRealAttribute("EW_Body_Weight")
Catch ex As Exception
bWeight = 0
End Try
Dim aNum As Double? = GetMaterialThickness(aMat)
Dim bNum As Double? = GetMaterialThickness(bMat)
' Handling primary sort based on EW_Material attribute
If aNum.HasValue And bNum.HasValue Then
primaryResult = bNum.Value.CompareTo(aNum.Value) ' Sort in descending order
ElseIf aNum.HasValue Then
primaryResult = -1
ElseIf bNum.HasValue Then
primaryResult = 1
Else
primaryResult = String.Compare(aMat, bMat) ' Sort alphabetically in that case
End If
' Handling secondary sort based on EW_Body_Weight attribute
If primaryResult = 0 Then
Return bWeight.CompareTo(aWeight) ' Sort in descending order based on weight
Else
Return primaryResult ' Otherwise, return the result of the primary comparison
End If
End Function)
Catch ex As Exception
lw.WriteLine(" ")
lw.WriteLine("Hoist the colors, we're navigating choppy seas... a fault has been discovered: " & ex.Message)
End Try
Else
Try
dispObj.Sort(Function(a, b)
Dim aMat As String = If(GetMaterialName(a) = "Not specified", "zzzzz", GetMaterialName(a))
Dim bMat As String = If(GetMaterialName(b) = "Not specified", "zzzzz", GetMaterialName(b))
Dim aNumVal As Double? = GetMaterialThickness(aMat)
Dim bNumVal As Double? = GetMaterialThickness(bMat)
' Compare numerical values if both are present
If aNumVal.HasValue AndAlso bNumVal.HasValue Then
Dim numCompare As Integer = bNumVal.Value.CompareTo(aNumVal.Value)
If numCompare <> 0 Then Return numCompare
ElseIf aNumVal.HasValue Then
Return -1
ElseIf bNumVal.HasValue Then
Return 1
End If
' If numerical values are equal or not present, compare the rest of the material name
Dim restCompare As Integer = String.Compare(aMat, bMat)
If restCompare <> 0 Then Return restCompare
' If materials are identical, compare weights
Dim aWeight As Double = GetBodyWeight(a)
Dim bWeight As Double = GetBodyWeight(b)
Return bWeight.CompareTo(aWeight) ' Sort by weight in descending order
End Function)
Catch ex As Exception
lw.WriteLine(" ")
lw.WriteLine("Ahoy, deckhands, a squall's upon us... an anomaly has presented itself: " & ex.Message)
End Try
End If
lw.WriteLine(" - Selected bodies captured and the Selection order: Sorted.")
Else
lw.WriteLine(" - Selected bodies captured and the Selection order: Preserved.")
End If
Return True ' Successfully selected and sorted objects
Else
' Handle the case where no objects are selected
lw.WriteLine("The chronicle paused, as no items were marked for the journey.")
Return False
End If
Else
lw.WriteLine(" ")
lw.WriteLine("Arr, what's this? A baffling response during the selection of the bounty: " & resp.ToString())
Return False
End If
End Function
Sub UpdateBodyWeight(ByVal body As Body)
Dim myMeasure As MeasureManager = workPart.MeasureManager
Dim massUnits(1) As Unit
massUnits(0) = workPart.UnitCollection.GetBase("Volume")
Dim mb As MeasureBodies = myMeasure.NewMassProperties(massUnits, 0.99, New Body() {body})
' Update the InformationUnit for MeasureBodies based on unit system
Dim informationUnit As MeasureBodies.AnalysisUnit
If unitString = "in" Then
mb.informationUnit = MeasureBodies.AnalysisUnit.PoundInch
Else
mb.informationUnit = MeasureBodies.AnalysisUnit.KilogramMilliMeter
End If
' Extract volume
Dim bodyVolume As Double = mb.Volume
mb.Dispose()
' Extract density from the EW_Material_Density attribute; default to 1 if not found
Dim density As Double = 1.0
Try
density = Convert.ToDouble(body.GetStringAttribute("EW_Material_Density"))
Catch ex As Exception
' If the attribute is not found or cannot be converted, use the default density of 1
'lw.WriteLine("Density attribute not found or invalid for body: " & body.JournalIdentifier & ". Using default density of 1.")
End Try
If unitString = "in" Then
' Calculate weight assuming density is in Pound/Cubic Foot, converting to lbm
Dim bodyWeight As Double = bodyVolume / 1728 * density
Try
body.SetUserAttribute("EW_Body_Weight", -1, bodyWeight, Update.Option.Now)
'lw.WriteLine("Updated EW_Body_Weight for: " & body.JournalIdentifier & " to " & bodyWeight.ToString("F3") & " Lbm")
Catch ex As Exception
'lw.WriteLine("Failed to update EW_Body_Weight for: " & body.JournalIdentifier & ". Error: " & ex.Message)
End Try
Else
' Calculate weight assuming density is in Kg/Cubic Meter, converting to kg
Dim bodyWeight As Double = bodyVolume / 1000000000.0 * density
Try
body.SetUserAttribute("EW_Body_Weight", -1, bodyWeight, Update.Option.Now)
'lw.WriteLine("Updated EW_Body_Weight for body: " & body.JournalIdentifier & " to " & bodyWeight.ToString("F3") & " Kg")
Catch ex As Exception
'lw.WriteLine("Failed to update EW_Body_Weight for body: " & body.JournalIdentifier & ". Error: " & ex.Message)
End Try
End If
End Sub
Function GetMaterialName(body As Body) As String
' Retrieve the material name for the body
Dim matName As String = ""
Try
matName = body.GetStringAttribute("Material")
Catch ex As Exception
Return If(matName Is Nothing, matName, "Not specified")
End Try
Return matName
End Function
Function GetMaterialThickness(materialName As String) As Double?
' Try to extract numerical value
Dim pattern As String = "(\d+/\d+)|(\d+(\.\d+)?)"
Dim matches As MatchCollection
Dim thickness As Double? = Nothing
Dim numericPart As String
If materialName.Contains(ssunitmm) Then
numericPart = materialName.Substring(0, materialName.IndexOf(ssunitmm)).Trim()
matches = Regex.Matches(numericPart, pattern)
'lw.WriteLine("Material name trimed (" & ssunitmm & ") : " & numericPart.ToString())
ElseIf materialName.Contains(ssunitin) Then
numericPart = materialName.Substring(0, materialName.IndexOf(ssunitin)).Trim()
matches = Regex.Matches(numericPart, pattern)
'lw.WriteLine("Material name trimed (" & ssunitin & ") : " & numericPart.ToString())
Else
matches = Regex.Matches(materialName, pattern)
End If
For Each match As Match In matches
If match.Success Then
Dim value As Double
If match.Value.Contains("/") Then
Dim parts As String() = match.Value.Split("/")
If parts.Length = 2 Then
Dim numerator As Double
Dim denominator As Double
If Double.TryParse(pa
(I was too focused on making this part fully custom). Apologies for that! If anyone reading this, you don’t need to go deep into the journal—everything has an option in the Configuration Settings.
