Community
The short answer:
- for the iProperties look at this blogpost:
- for the material have a look at this post:
- for the QTY i have to disapoint you. it can be done but have a look at this posts:
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:
Jelte de Jong
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Blog: hjalte.nl - github.com
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? 🙂
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.NameDim Material As String = oRefDoc.ActiveMaterial.DisplayName
Jelte de Jong
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Blog: hjalte.nl - github.com
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").
Jelte de Jong
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Blog: hjalte.nl - github.com
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
