iLogic: replace item number with filename (3D Template)
Just to be clear...this is an Assembly File Template, right?
Does this template file already have items in it to start with, as part of the template?
The items in the BOM in the image appear to be Multi-Body Part files, so I asume you are wanting each component within this main assembly to be named something like: = oAssemblyFileName & " - " & oOccuranceNumber, right?
If so, this definately sounds doable, asuming it will accept a String type data instead of Integer.
I could give it a try if you'd like.
Wesley Crihfield
(Not an Autodesk Employee)
Try the following iLogic code:
Dim oAdoc As AssemblyDocument oAdoc = ThisApplication.ActiveDocument Dim oCompDef As AssemblyComponentDefinition oCompDef = oAdoc.ComponentDefinition Dim oBOM As BOM oBOM = oCompDef.BOM oBOM.StructuredViewEnabled = True Dim oBOMviews As BOMViews oBOMviews = oBOM.BOMViews Dim oBOMview As BOMView Dim oBOMrows As BOMRowsEnumerator Dim oBOMrow As BOMRow 'Define this assembly's File Name Dim oAFN As String oAFN = ThisDoc.FileName(False) i = 1 For Each oBOMview In oBOMviews If oBOMview.ViewType = BOMViewTypeEnum.kStructuredBOMViewType Then oBOMrows = oBOMview.BOMRows For Each oBOMrow In oBOMrows oBOMrow.ItemNumber = oAFN & " - " & i.ToString Next End If Next
I hope this helps.
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Wesley Crihfield
(Not an Autodesk Employee)
OK. I need to further clarify before doing more coding.
Within this image, it appears that you intend to have every Item Number be exactly the same as the Part Number on the same row. Do you want both the Part Number & the Item Number edited to make this happen? Both can be edited within the BOM, but I don't know if this may cause you problems later or not. Is each line item's Part Number already exactly the same as its File Name, before any code is ran? If you just want the Item Number of each Row to be exactly the same as that Row's Part Number, and there were multiple line items with the same part number, you'd have to add something to the end of the item number, or it will give an error and not work. Each line item within the BOM must have a unique Item Number.
Wesley Crihfield
(Not an Autodesk Employee)
OK. Try This.
Dim oAdoc As AssemblyDocument
oAdoc = ThisApplication.ActiveDocument
Dim oCompDef As AssemblyComponentDefinition
oCompDef = oAdoc.ComponentDefinition
Dim oUParams As UserParameters
oUParams = oCompDef.Parameters.UserParameters
Dim oParamName As String
oParamName = "ReplaceItemNumber"
Dim oExists As Boolean
oExists = False
For Each oUParam As UserParameter In oUParams
If oUParam.Name = oParamName Then
oExists = True
End If
Next
If oExists = False Then
'The specified Parameter doesn't exist, so create it, sets its value(s) & options.
oParameter = oUParams.AddByExpression(oParamName, False ,UnitsTypeEnum.kBooleanUnits)
Parameter.Param(oParamName).IsKey = True
ElseIf oExists = True Then
oAnswer = MessageBox.Show("Do you want to replace the Item Numbers within the BOM?","BOM ITEM NUMBERS",MessageBoxButtons.YesNo,MessageBoxIcon.Question,MessageBoxDefaultButton.Button2)
If oAnswer = vbNo Then
Parameter(oParamName) = False
ElseIf oAnswer = vbYes Then
Parameter(oParamName) = True
End If
End If
Dim oBOM As BOM
oBOM = oCompDef.BOM
oBOM.StructuredViewEnabled = True
Dim oItemCompDef As ComponentDefinition
Dim oItemPN As [Property]
If Parameter(oParamName) = True Then
i = 1
For Each oBOMview As BOMView In oBOM.BOMViews
If oBOMview.ViewType = BOMViewTypeEnum.kStructuredBOMViewType Then
For Each oBOMrow As BOMRow In oBOMview.BOMRows
oItemCompDef = oBOMrow.ComponentDefinitions.Item(1)
If TypeOf oItemCompDef Is AssemblyComponentDefinition Then
oItemPN = oItemCompDef.Document.PropertySets.Item("Design Tracking Properties").Item("Part Number")
oBOMrow.ItemNumber = oItemPN
End If
Next
End If
Next
End If
Wesley Crihfield
(Not an Autodesk Employee)
OK. I think I've corrected the problem now. Try this.
Dim oAdoc As AssemblyDocument
oAdoc = ThisApplication.ActiveDocument
Dim oCompDef As AssemblyComponentDefinition
oCompDef = oAdoc.ComponentDefinition
Dim oUParams As UserParameters
oUParams = oCompDef.Parameters.UserParameters
Dim oParamName As String
oParamName = "ReplaceItemNumber"
Dim oExists As Boolean
oExists = False
For Each oUParam As UserParameter In oUParams
If oUParam.Name = oParamName Then
oExists = True
End If
Next
If oExists = False Then
'The specified Parameter doesn't exist, so create it, sets its value(s) & options.
oParameter = oUParams.AddByValue(oParamName, "False", UnitsTypeEnum.kTextUnits)
MultiValue.SetList(oParamName,"True","False")
Parameter.Param(oParamName).IsKey = True
ElseIf oExists = True Then
oAnswer = MessageBox.Show("Do you want to replace the Item Numbers within the BOM?","BOM ITEM NUMBERS",MessageBoxButtons.YesNo,MessageBoxIcon.Question,MessageBoxDefaultButton.Button2)
If oAnswer = vbNo Then
Parameter(oParamName) = "False"
ElseIf oAnswer = vbYes Then
Parameter(oParamName) = "True"
End If
End If
Dim oBOM As BOM
oBOM = oCompDef.BOM
oBOM.StructuredViewEnabled = True
Dim oItemPN As [Property]
If Parameter(oParamName) = "True" Then
i = 1
For Each oBOMview As BOMView In oBOM.BOMViews
If oBOMview.ViewType = BOMViewTypeEnum.kStructuredBOMViewType Then
For Each oBOMrow As BOMRow In oBOMview.BOMRows
If oBOMrow.ReferencedFileDescriptor.ReferencedFileType = FileTypeEnum.kAssemblyFileType Then
For Each oDoc As Document In oAdoc.AllReferencedDocuments
If oDoc.FullFileName = oBOMrow.ReferencedFileDescriptor.FullFileName Then
oItemPN = oDoc.PropertySets.Item("Design Tracking Properties").Item("Part Number")
oBOMrow.ItemNumber = oItemPN.Value.ToString
End If
Next
End If
Next
End If
Next
End If
Wesley Crihfield
(Not an Autodesk Employee)
This version will deal with "ChildRows" of the main BOM rows too.
There are a couple other variables that this rule identifies and notifies you of, but doesn't do anything with at this point, because I don't know if you have any of these within your BOM.
These variables are:
- If the row is "Merged"
- If the row is "Promoted"
- If the row is "RolledUp"
Right now I have just set-up a MessageBox to tell you if one of these conditions is true of the BOM row.
As for the triggering, of the rule to run when the Parameter value changes, this can be done in a few different ways.
Simply using the Manage tab / iLogic panel / Event Triggers tool, most likely won't work for this rule, because it is a UserParameter and not a ModelParameter, for one, and it is a Text type parameter secondly. Also it wouldn't be a good idea to use the iProperty Change trigger in those settings unless you have a rule which converts your Text & Boolean style parameters to Custom iProperties (which is easy to do).
I think the best two options for firing this rule would be the following:
- If you are changing the "ReplaceItemNumber" parameter manually from a Form, you could unclude a button below that within your form, that runs this rule.
- If you are changing the "ReplaceItemNumber" parameter manually from the Parameters dialog box, then you should create a local rule within the document, that contains a RunExternalRule("RuleName") line. Then above that line, create a line something like oDummyVariable1 = ReplaceItemNumber. The parameter name should not be in quotation marks, it should be blue (the default color code for local parameters). This causes the file to 'watch' that local parameter for changes, then run the rule when it does.
Wesley Crihfield
(Not an Autodesk Employee)
Forgot to insert the code:
Dim oAdoc As AssemblyDocument
oAdoc = ThisApplication.ActiveDocument
Dim oCompDef As AssemblyComponentDefinition
oCompDef = oAdoc.ComponentDefinition
Dim oUParams As UserParameters
oUParams = oCompDef.Parameters.UserParameters
Dim oParamName As String
oParamName = "ReplaceItemNumber"
Dim oExists As Boolean
oExists = False
For Each oUParam As UserParameter In oUParams
If oUParam.Name = oParamName Then
oExists = True
End If
Next
If oExists = False Then
'The specified Parameter doesn't exist, so create it, sets its value(s) & options.
oParameter = oUParams.AddByValue(oParamName, "False", UnitsTypeEnum.kTextUnits)
MultiValue.SetList(oParamName,"True","False")
Parameter.Param(oParamName).IsKey = True
ElseIf oExists = True Then
oAnswer = MessageBox.Show("Do you want to replace the Item Numbers within the BOM?","BOM ITEM NUMBERS",MessageBoxButtons.YesNo,MessageBoxIcon.Question,MessageBoxDefaultButton.Button2)
If oAnswer = vbNo Then
Parameter(oParamName) = "False"
ElseIf oAnswer = vbYes Then
Parameter(oParamName) = "True"
End If
End If
Dim oBOM As BOM
oBOM = oCompDef.BOM
oBOM.StructuredViewEnabled = True
Dim oItemPN As [Property]
Dim oChildItemPN As [Property]
Dim oDoc As Document
If Parameter(oParamName) = "False" Then
Return
ElseIf Parameter(oParamName) = "True" Then
i = 1
For Each oBOMview As BOMView In oBOM.BOMViews
If oBOMview.ViewType = BOMViewTypeEnum.kStructuredBOMViewType Then
For Each oBOMrow As BOMRow In oBOMview.BOMRows
If oBOMrow.ReferencedFileDescriptor.ReferencedFileType = FileTypeEnum.kAssemblyFileType Then
If oBOMrow.Merged = True Then
MessageBox.Show("This BOM row: " & oBOMrow.ItemNumber & " has been 'Merged'.")
End If
If oBOMrow.Promoted = True Then
MessageBox.Show("This BOM row: " & oBOMrow.ItemNumber & " has been 'Promoted'.")
End If
If oBOMrow.RolledUp = True Then
MessageBox.Show("This BOM row: " & oBOMrow.ItemNumber & " has been 'RolledUp'.")
End If
If oBOMrow.ChildRows.Count > 0 Then
For Each oChildRow As BOMRow In oBOMrow.ChildRows
For Each oDoc In oAdoc.AllReferencedDocuments
If oDoc.FullFileName = oChildRow.ReferencedFileDescriptor.FullFileName Then
oChildItemPN = oDoc.PropertySets.Item("Design Tracking Properties").Item("Part Number")
oChildRow.ItemNumber = oChildItemPN.Value.ToString
End If
Next
Next
End If
If oBOMrow.ChildRows Is Nothing Then
For Each oDoc In oAdoc.AllReferencedDocuments
If oDoc.FullFileName = oBOMrow.ReferencedFileDescriptor.FullFileName Then
oItemPN = oDoc.PropertySets.Item("Design Tracking Properties").Item("Part Number")
oBOMrow.ItemNumber = oItemPN.Value.ToString
End If
Next
End If
End If
Next
End If
Next
End If
Wesley Crihfield
(Not an Autodesk Employee)
