Upgrading Export DXF flat pattern from Assembly with iProperty naming

[vkulikajevas]

I need to Use this Rule (Or similar) to generate flat patterns from assembly sheet files. Problem is I can't figure it out how to make this rule to name all created DXF files to using every part info:
Description (From the sheet part) & " "  & Material (From the sheet part) & " " Stock Number (From the sheet part) " " QTY (From the assembly - i.d. QTY used in assembly of each part).

'define the active document as an assembly file
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisApplication.ActiveDocument
oAsmName = Left(oAsmDoc.DisplayName, Len(oAsmDoc.DisplayName) -4)
'check that the active document is an assembly file
If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then
MessageBox.Show("Please run this rule from the assembly file.", "iLogic")
Exit Sub
End If
'get user input
RUsure = MessageBox.Show ( _
"This will create a DXF file for all of the asembly components that are sheet metal." _
& vbLf & "This rule expects that the part file is saved." _
& vbLf & " " _
& vbLf & "Are you sure you want to create DXF for all of the assembly components?" _
& vbLf & "This could take a while.", "iLogic - Batch Output DXFs ",MessageBoxButtons.YesNo)
If RUsure = vbNo Then
Return
Else
End If
oPath = ThisDoc.Path
oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
oContext = ThisApplication.TransientObjects.CreateTranslationContext
oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
oOptions = ThisApplication.TransientObjects.CreateNameValueMap
'get DXF target folder path
oFolder = oPath & "\" & oAsmName & " DXF Files"
'Check for the DXF folder and create it if it does not exist
If Not System.IO.Directory.Exists(oFolder) Then
System.IO.Directory.CreateDirectory(oFolder)
End If
'- - - - - - - - - - - - -'- - - - - - - - - - - - -Component - - - - - - - - - - - -'look at the files referenced by the assembly
Dim oRefDocs As DocumentsEnumerator
oRefDocs = oAsmDoc.AllReferencedDocuments
Dim oRefDoc As Document
'work the the drawing files for the referenced models'this expects that the model has been saved
For Each oRefDoc In oRefDocs
iptPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) - 3) & "ipt"
'check that model is saved
If(System.IO.File.Exists(iptPathName)) Then
Dim oDrawDoc As PartDocument
oDrawDoc = ThisApplication.Documents.Open(iptPathName, True)
oFileName = Left(oRefDoc.DisplayName, Len(oRefDoc.DisplayName))
Try
'Set the DXF target file name

Try
CustomName =iProperties.Value(oFileName, "Custom", "PF_PRT_ZNR")
Catch
CustomName ="XXX" 'Wert, wenn iPropertie PF_PRT_ZNR nicht existiert
End Try

oDataMedium.FileName = oFolder & "\" & CustomName  & " " & oFileName & ".dxf"

Dim oCompDef As SheetMetalComponentDefinition
oCompDef = oDrawDoc.ComponentDefinition
If oCompDef.HasFlatPattern = False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut = "FLAT PATTERN DXF?AcadVersion=2004&OuterProfileLayer=IV_OUTER_PR?OFILE"
oCompDef.DataIO.WriteDataToFile( sOut, oDataMedium.FileName)
'just for check its works coretcly'i=MessageBox.Show(oDataMedium.FileName, "Title",MessageBoxButtons.OKCancel)'MessageBox.Show(i,"title",MessageBoxButtons.OK)'If i=2 Then'Exit Sub'End If
oCompDef.FlatPattern.ExitEdit
Catch
End Try
oDrawDoc.Close
Else
End If
Next

[JelteDeJong · Accepted solution]

The short answer:

• for the iProperties look at this blogpost:
  • https://modthemachine.typepad.com/my_weblog/2010/02/accessing-iproperties.html
• for the material have a look at this post:
  • https://forums.autodesk.com/t5/inventor-customization/sheet-metal-style-material/m-p/2354776/highlig...
• for the QTY i have to disapoint you. it can be done but have a look at this posts:
  
  • https://adndevblog.typepad.com/manufacturing/2013/12/bom-item-total-quantity-by-sub-assemby.html
  • https://forums.autodesk.com/t5/inventor-customization/how-to-get-the-total-occurrences-in-active-doc...

long aswer i did have a look at your code. i implemented the properties en material in the filename of the dxf.

Also i found a a couple of things that could be done better. I added comments to the code and  changed it in a way i think is better.

'check that the active document is an assembly file
        '--> first check if the is an assembly before you declare it to an AssemblyDocument
        If ThisApplication.ActiveDocument.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
            MessageBox.Show("Please run this rule from the assembly file.", "iLogic")
            Exit Sub
        End If

        'define the active document as an assembly file
        Dim oAsmDoc As AssemblyDocument = ThisApplication.ActiveDocument
        '--> oAsmDoc.DisplayName can show the extension depending on windows settings.
        '--> i guess that you try to remove the extensin here.
        '--> if you do it in this way your colega, with different windows settings, will have an unexpexted resilt. 
        'Dim oAsmName = Left(oAsmDoc.DisplayName, Len(oAsmDoc.DisplayName) - 4)
        Dim oAsmName = oAsmDoc.DisplayName.Replace(".iam", "")


        'get user input
        Dim RUsure = MessageBox.Show(
"This will create a DXF file for all of the asembly components that are sheet metal." _
& vbLf & "This rule expects that the part file is saved." _
& vbLf & " " _
& vbLf & "Are you sure you want to create DXF for all of the assembly components?" _
& vbLf & "This could take a while.", "iLogic - Batch Output DXFs ", MessageBoxButtons.YesNo)
        If RUsure = vbNo Then
            Return
            ' Else <-- this is not needed.
        End If

        Dim oPath = ThisDoc.Path

        '--> it seems that you use oDataMedium only for the file path.
        '--> you might want to have a look at the k.i.s.s. design principl 
        '--> https://en.wikipedia.org/wiki/KISS_principle
        '--> i think you wont need it.
        'Dim oDataMedium = ThisApplication.TransientObjects.CreateDataMedium

        '--> oContext is declared her but is never used...
        'Dim oContext = ThisApplication.TransientObjects.CreateTranslationContext
        'oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism

        '--> oOptions is declared her but is never used...
        'Dim oOptions = ThisApplication.TransientObjects.CreateNameValueMap

        'get DXF target folder path
        Dim oFolder = oPath & "\" & oAsmName & " DXF Files"
        'Check for the DXF folder and create it if it does not exist
        If Not System.IO.Directory.Exists(oFolder) Then
            System.IO.Directory.CreateDirectory(oFolder)
        End If
        '- - - - - - - - - - - - -'- - - - - - - - - - - - -Component - - - - - - - - - - - -
        'look at the files referenced by the assembly
        Dim oRefDocs As DocumentsEnumerator = oAsmDoc.AllReferencedDocuments

        'work the the drawing files for the referenced models'this expects that the model has been saved
        For Each oRefDoc As Document In oRefDocs

            '--> this seem to replase the extension of the filename. Then you try to check with this 
            '--> if it is saved (and probaly if its an part and not an assembly)
            '--> you can better use the Document.Dirty property. this will be false if the file is not saved.
            '--> also if the file exists but was not saved.
            '--> for checking if its a part we can use the Document.DocumentType.
            '--> last i did not see if you checked if it is realy a sheet metal part. 
            '--> we can do that with the Document.SubType

            'Dim iptPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) - 3) & "ipt"
            'check that model is saved
            'If (System.IO.File.Exists(iptPathName)) Then

            '--> check if its a part:
            If (oRefDoc.DocumentType <> DocumentTypeEnum.kPartDocumentObject) Then
                Continue For '--> this will make the program go to the next oRefDoc
            End If
            '--> check if its a Sheetmetal part:
            If (oRefDoc.SubType <> "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then
                Continue For '--> this will make the program go to the next oRefDoc
            End If
            '--> check if its saved:
            If (oRefDoc.Dirty = True) Then
                '--> TODO ask the user if he/she wants to save?
                '--> oRefDoc.Save()
                Continue For '--> this will make the program go to the next oRefDoc
            End If

            Dim oDrawDoc As PartDocument = ThisApplication.Documents.Open(oRefDoc.FullFileName, True)
            Dim oFileName = oRefDoc.DisplayName.Replace(".ipt", "")
            Dim oCompDef As SheetMetalComponentDefinition = oDrawDoc.ComponentDefinition
            Try
                'Set the DXF target file name
                '--> you need to declare the CustomName before the try/cath or you will only be able to use its value in try/cath statement
                '--> i also declared the other values that you asked for. (with there default values so i dont have to do it in the cath block) 
                Dim customPropertiesSet = oRefDoc.PropertySets.Item("Inventor User Defined Properties")
                Dim customName As String = "XXX"
                Try
                    customName = customPropertiesSet.Item("PF_PRT_ZNR").Value
                Catch
                    '--> TODO create a msgbox to want the user that the name can be starnge
                    'customName = "XXX" 'Wert, wenn iPropertie PF_PRT_ZNR nicht existiert
                End Try

                Dim designTrackingPropertiesSet = oRefDoc.PropertySets.Item("Design Tracking Properties")
                Dim description As String = designTrackingPropertiesSet.Item("Description").Value
                Dim StockNumber As String = designTrackingPropertiesSet.Item("Stock Number").Value

                Dim Material As String = oCompDef.ActiveSheetMetalStyle.Material.Name

                'oDataMedium.FileName = oFolder & "\" & CustomName & " " & oFileName & ".dxf"
                Dim newFileName As String =
                    oFolder & "\" & customName & " " & description & " " & StockNumber & " " & Material & ".dxf"


                If oCompDef.HasFlatPattern = False Then
                    oCompDef.Unfold()
                Else
                    oCompDef.FlatPattern.Edit()
                End If
                Dim sOut As String
                sOut = "FLAT PATTERN DXF?AcadVersion=2004&OuterProfileLayer=IV_OUTER_PR?OFILE"
                oCompDef.DataIO.WriteDataToFile(sOut, newFileName)
                'oCompDef.DataIO.WriteDataToFile(sOut, oDataMedium.FileName)
                oCompDef.FlatPattern.ExitEdit()
            Catch
            End Try
            oDrawDoc.Close()
            'Else
            'End If
        Next

:

[vkulikajevas]

The code works really well! Thank you very much!

[vkulikajevas]

JelteDeJong, there is something wrong with the code when writing material to the parts.

It always writes AISI 304 instead of material that I applied to parts. Maybe you could have a fix for that? 🙂

[JelteDeJong]

My code does work but maby not as you expected probaly. It's a bit confusing but for sheetmetal parts the matrial that you can select in the top of your screen is an override from the material in the sheetmatal rules. I think it's best to use the sheetmatal rules to set the material because then it's possible to also set material thickness, k-factor's, and other stuff that is importend for sheetmetal parts in 1 click.

That being said if you want to use the override then change the code that get the material in this:

'Dim Material As String = oCompDef.ActiveSheetMetalStyle.Material.Name
Dim Material As String = oRefDoc.ActiveMaterial.DisplayName

[aurel_e]

@JelteDeJong 

Is there any way to run this ilogic rule "silently"? I mean without opening every sheet metal file. Actually it opens them save the flat pattern and close them. Can we change the code to make it run in background? 

[aurel_e]

I think I figured it out 

oDrawDoc = ThisApplication.Documents.Open(iptPathName, True) -> False

[aurel_e]

Another question: is it possible to set the dxf layers? For instance: I would like to have the UNCONSUMED SKETCHES layer name Yellow, color Yellow.

[JelteDeJong]

hi it's possible you will need to change the option string (sOut). in your script replace the line:

sOut = "FLAT PATTERN DXF?AcadVersion=2004&OuterProfileLayer=IV_OUTER_PR?OFILE"

with (see also comments in code):

Dim optionList As List(Of String) = New List(Of String)()

optionList.add("AcadVersion=2004")
optionList.add("OuterProfileLayer=IV_OUTER_PR")
optionList.add("UnconsumedSketchesLayerColor=255;0;0") 'here i make the UnconsumedSketchesLayer lines red!
optionList.add("") 'you can add other options here
optionList.add("") 'and more options
' if you want you can add more lines for more options

Dim sOut As String
sOut = "FLAT PATTERN DXF?"
For Each opt In optionList
	sOut = sOut & "&" & opt
Next
sOut = sOut & "?OFILE"

in the new code you can add option like they are discribed in the help files (search for: "Translate - Sheet Metal to DXF API Sample").

[aurel_e]

@JelteDeJong  Thank you very much.

It works. This is the final part of my rule: 

oCompDef = oDrawDoc.ComponentDefinition

Dim optionList As List(Of String) = New List(Of String)()

optionList.Add("AcadVersion=2004")
optionList.Add("OuterProfileLayer=0")
optionList.Add("InteriorProfilesLayer=0")
optionList.Add("UnconsumedSketchesLayer=YELLOW")
optionList.add("UnconsumedSketchesLayerColor=255;255;0") 'here i make the UnconsumedSketchesLayer lines red!

Dim sOut As String
sOut = "FLAT PATTERN DXF?AcadVersion=2000" _
+ "&InvisibleLayers=IV_TANGENT;IV_FEATURE_PROFILES_D​OWN;IV_ARC_CENTERS;IV_BEND;IV_BEND_DOWN;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_FEATURE_PROFILES;	IV_FEATURE_PROFILES_DOWN" 

 
For Each opt In optionList
	sOut = sOut & "&" & opt
Next
sOut = sOut & "?OFILE"
oCompDef.DataIO.WriteDataToFile( sOut, oDataMedium.FileName)

oCompDef.FlatPattern.ExitEdit
Catch
End Try
oDrawDoc.Close
Else
End If
Next

[aurel_e]

@JelteDeJong 

Something is not working properly:

I have an assembly with some Ipt that are derived parts. The code is exporting the derived part sources  as well.

Can we make the code to avoid it?

I would like the code to export just the components in this LOD, ignoring the suppressed parts as well.

Thank you.

[Anonymous]

I have assembly contain sub assembly, how can activate every part (as I assembly) inside this assembly or sub assembly and export dxf for each sheet metal parts

[ricky_galetaSGGSQ]

this code seems to be skipping a few parts and i have no idea why ?