Export assembly as individual step files

[Anonymous]

Hi all,

I am able to export the assembly as one step file with the full model tree but I am trying to export an assembly into individual step files of every component in that assembly, is there any way to do this easily?

Cheers,

Iain

[Roelof.Feijen]

Hi Iain,

I don't think you can do this in Inventor without customization.

NXTdim Batch Publish van do it. You can download a trial form the Inventor Exchange

https://apps.autodesk.com/en/Publisher/PublisherHomepage?ID=HUSPL4JKGND7

Otherwise you need to write your own VBA or iLogic rule to do this.

[Anonymous]

Hi Roelof,

Thank you for your reply, is there anywhere I can look for guidance on creating an ilogic rule to do this?

Iain

[mdavis22569]

Look at your Task Scheduler ...

It has an Export option. You can do all of the files in an IPJ.. 

Might need to tweak it a bit

[Anonymous]

Hi Michael,

I used Task Scheduler in the end but it wasn't ideal because all the files were in several different folders and not necessarily all the files in that folder either.

What I really want is for all the components visible in the model view of an assembly to be exported, I am currently trying to write an illogic script to do just that.

Cheers,

Iain

[Justin.Williams]

I have been using the iLogic code provided in the link below to export PDF files of drawings for each component in an assembly. 

I bet this code can be modified to make it export .stp instead of a PDF of the drawing. I wish I knew how, because this is something I also want to be able to do. I currently use task scheduler and select each component manually and change the export option to .stp one at a time. 

Does anyone know how to modify it to make it export .stp?

http://inventortrenches.blogspot.com/2012/11/ilogic-batch-output-pdfs-from-assembly.html

'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 PDF file for all of the asembly components that have drawings files." _
& vblf & "This rule expects that the drawing file shares the same name and location as the component." _
& vblf & " " _
& vblf & "Are you sure you want to create PDF Drawings for all of the assembly components?" _
& vblf & "This could take a while.", "iLogic  - Batch Output PDFs ",MessageBoxButtons.YesNo)

If RUsure = vbNo Then
Return
Else
End If

'- - - - - - - - - - - - -PDF setup - - - - - - - - - - - -
oPath = ThisDoc.Path
PDFAddIn = ThisApplication.ApplicationAddIns.ItemById("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}")
oContext = ThisApplication.TransientObjects.CreateTranslationContext
oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
oOptions = ThisApplication.TransientObjects.CreateNameValueMap
oDataMedium = ThisApplication.TransientObjects.CreateDataMedium

If PDFAddIn.HasSaveCopyAsOptions(oDataMedium, oContext, oOptions) Then
'oOptions.Value("All_Color_AS_Black") = 0
oOptions.Value("Remove_Line_Weights") = 1
oOptions.Value("Vector_Resolution") = 400
oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets
'oOptions.Value("Custom_Begin_Sheet") = 2
'oOptions.Value("Custom_End_Sheet") = 4
End If

'get PDF target folder path
oFolder = oPath & "\" & oAsmName & " PDF Files"

'Check for the PDF 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 Drawings - - - - - - - - - - - -
'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 a drawing of the same path and name
For Each oRefDoc In oRefDocs
idwPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) - 3) & "idw"
'check to see that the model has a drawing of the same path and name
If(System.IO.File.Exists(idwPathName)) Then
                        Dim oDrawDoc As DrawingDocument
                oDrawDoc = ThisApplication.Documents.Open(idwPathName, True)
            oFileName = Left(oRefDoc.DisplayName, Len(oRefDoc.DisplayName) -3)

            On error Resume Next ' if PDF exists and is open or read only, resume next
                 'Set the PDF target file name
                oDataMedium.FileName = oFolder & "\" & oFileName & "pdf"
                'Write out the PDF
                Call PDFAddIn.SaveCopyAs(oDrawDoc, oContext, oOptions, oDataMedium)
            'close the file
                oDrawDoc.Close
Else
'If the model has no drawing of the same path and name - do nothing
End If
Next
'- - - - - - - - - - - - -

'- - - - - - - - - - - - -Top Level Drawing - - - - - - - - - - - -
oAsmDrawing = ThisDoc.ChangeExtension(".idw")
oAsmDrawingDoc = ThisApplication.Documents.Open(oAsmDrawing, True)
oAsmDrawingName = Left(oAsmDrawingDoc.DisplayName, Len(oAsmDrawingDoc.DisplayName) -3)
'write out the PDF for the Top Level Assembly Drawing file
On error Resume Next ' if PDF exists and is open or read only, resume next
 'Set the PDF target file name
oDataMedium.FileName = oFolder & "\" & oAsmDrawingName & "pdf"
'Write out the PDF
Call PDFAddIn.SaveCopyAs(oAsmDrawingDoc, oContext, oOptions, oDataMedium)
'Close the top level drawing
oAsmDrawingDoc.Close
'- - - - - - - - - - - - -

MessageBox.Show("New Files Created in: " & vblf & oFolder, "iLogic")
'open the folder where the new ffiles are saved
Shell("explorer.exe " & oFolder,vbNormalFocus)

[salariua]

drawings as stp?

you mean assembly structure (parts and subcomponents to stp)?

it's not that difficult, will give it a stab.....

Oops....I've done it already, and forgot about it.

Check it here: http://blog.ads-sol.com/2016/01/batch-assembly-export.html

Good Luck.

[Justin.Williams · Accepted solution]

Thanks for sharing! That was helpful, but I need step files for ONLY files which have a drawing. I modified your code a bit so that it first checks to see if a file has a drawing, and if a drawing exists, it will export the step file.

Hopefully someone else finds it helpful! This will be a huge time saver for me

 '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 STP file for all of the asembly components that have drawings files." _
& vbLf & "This rule expects that the drawing file shares the same name and location as the component." _
& vbLf & " " _
& vbLf & "Are you sure you want to create PDF Drawings for all of the assembly components?" _
& vbLf & "This could take a while.", "iLogic  - Batch Output PDFs ",MessageBoxButtons.YesNo)

If RUsure = vbNo Then
Return
Else
End If

'- - - - - - - - - - - - -STEP setup - - - - - - - - - - - - 
oPath = ThisDoc.Path
'get STEP target folder path 
oFolder = oPath & "\" & oAsmName & " STEP Files"
'Check for the step 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 Drawings - - - - - - - - - - - -
'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 a drawing of the same path and name
For Each oRefDoc In oRefDocs
idwPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) - 3) & "idw"
'check to see that the model has a drawing of the same path and name
If(System.IO.File.Exists(idwPathName)) Then
                        Dim oDrawDoc As DrawingDocument
                oDrawDoc = ThisApplication.Documents.Open(idwPathName, True)
            oFileName = Left(oRefDoc.DisplayName, Len(oRefDoc.DisplayName) -3)

            On Error Resume Next ' if PDF exists and is open or read only, resume next
                 'Set the PDF target file name
                oDataMedium.FileName = oFolder & "\" & oFileName & "pdf"
                'Write out the PDF
                Call PDFAddIn.SaveCopyAs(oDrawDoc, oContext, oOptions, oDataMedium)
            'close the file
                oDrawDoc.Close
Else
'If the model has no drawing of the same path and name - do nothing
End If
Next
'- - - - - - - - - - - - -

'- - - - - - - - - - - - -Top Level Drawing - - - - - - - - - - - -
oAsmDrawing = ThisDoc.ChangeExtension(".idw")
oAsmDrawingDoc = ThisApplication.Documents.Open(oAsmDrawing, True)
oAsmDrawingName = Left(oAsmDrawingDoc.DisplayName, Len(oAsmDrawingDoc.DisplayName) -3)
'write out the PDF for the Top Level Assembly Drawing file
On Error Resume Next ' if PDF exists and is open or read only, resume next
 'Set the PDF target file name
oDataMedium.FileName = oFolder & "\" & oAsmDrawingName & "pdf"
'Write out the PDF
Call PDFAddIn.SaveCopyAs(oAsmDrawingDoc, oContext, oOptions, oDataMedium)
'Close the top level drawing
oAsmDrawingDoc.Close
'- - - - - - - - - - - - -

MessageBox.Show("New Files Created in: " & vbLf & oFolder, "iLogic")
'open the folder where the new ffiles are saved
Shell("explorer.exe " & oFolder,vbNormalFocus) 

[salariua]

Uhhh..... goodies 

I am soooo gonna be stealing your code now!

Brill find, keep up the good work @Justin.Williams

[Anonymous]

Thanks for all the responses! That code works miracles! I also found this thread from Feb '16 that looks to see if the file is part of the Normal BOM structure before export.

http://forums.autodesk.com/t5/inventor-forum/ilogic-to-export-step-from-marked-as-normal-in-bom/td-p...

Cheers,

Iain

[mazur_peter]

This post is a Great! 🙂
Thanks

Let me one question. If I want to add more data to a step file name (custom iProperties), how can I make it?
So I create a custom iProperty (i.e.: "comp_drawno") in a custom property tab. How can I add to the code to create the step file name with comp_drawno?

Many thanks

[Anonymous]

Could you please explain of how to fix the compile errors that occur .

I clicked on Add Rule, gave it a name(Rule) and pasted the code.

[Anonymous]

Hi guys,

I appreciate  your effort in providing a solution. Unfortunately, my problem goes a little further. Maybe one of you has an idea how to fix it.

I also need a way to export assemblies as STEP files with individual files for each of the assembly's components.

However, in the end I want the STEP-file of the assembly to only contain references to the components' files but not the entire assembly's geometry.

In creo parametric there is such an option.

The reason we need this is that our own software is capable of importing step data. If we or our customers were able to sort out certain components such as standard parts in the windows explorer, the imported models would be much leaner, increasing our software's performance.

If you could think of any way to establish such a procedure, I would really appreciate any hint.

Thank you! Cheers, Malte Vollmer

[johnsonshiue]

Hi! I think I know what you are talking about. But, I don't think Inventor supports such STEP Export workflow. I need to work with the project team to understand the request better and how we can accommodate it.

Many thanks!

[johnsonshiue]

Hi! I got confirmation from the project team that the distributed STEP files are not yet supported. Please submit it as an idea to Inventor Ideas forum (https://forums.autodesk.com/t5/inventor-ideas/idb-p/v1232).

Many thanks!

[Anonymous]

Hi, I am trying to use this iLogic rule to export PDF's and STEP files of my assembly. There are a plethora of errors with Inventor 2018. Is there an updated rule I can use? I don't understand much about iLogic rules other than how to add them.

[dliteful]

This is what I was able to come up with for PDF & STEP files.  Works good, but I can imagine it would take a while with larger assemblies.  This was created in Inventor 2017, so I hope there are not 2018 bugs for you.

Sub Main()
    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
    If MessageBox.Show ( _
        "This will create a PDF & STEP file for all of the assembly components that have drawings files." _
        & vbLf & "This rule expects that the drawing file shares the same name and location as the component." _
        & vbLf & " " _
        & vbLf & "Are you sure you want to create these files for all of the assembly components?" _
        & vbLf & "This could take a while.", "iLogic  - Batch Output STPs ",MessageBoxButtons.YesNo) = vbNo Then
        
        Exit Sub
    End If
        
    Dim PDFAddIn As TranslatorAddIn
    Dim oContext As TranslationContext
    Dim oOptions As NameValueMap
    Dim oDataMedium As DataMedium
    
    Call ConfigurePDFAddinSettings(PDFAddIn, oContext, oOptions, oDataMedium)
    
    oPath = ThisDoc.Path
    oFolder = oPath & "\_" & oAsmName & " PDF & STEP Files"
    
    If Not System.IO.Directory.Exists(oFolder) Then
        System.IO.Directory.CreateDirectory(oFolder)
    End If
    
    '- - - - - - - - - - - - -Component Drawings - - - - - - - - - - - -'
    'look at the files referenced by the assembly
    Dim oRefDoc As Document
    
    For Each oRefDoc In oAsmDoc.AllReferencedDocuments
        idwPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentNaMe) - 3) & "idw"

        If(System.IO.File.Exists(idwPathName)) Then
            Dim oDrawDoc As DrawingDocument
            oDrawDoc = ThisApplication.Documents.Open(idwPathName, True)
            Dim oSTEPDoc As Document
            oSTEPDoc = ThisApplication.Documents.Open(oRefDoc.FullFileName, True)
            oFileName = Left(oRefDoc.DisplayName, Len(oRefDoc.DisplayName) -4)
            oRevNum = oDrawDoc.PropertySets.Item("Inventor Summary Information").Item("Revision Number").Value
'            On Error Resume Next
'            'Set the PDF target file name
                If oRevNum = Nothing Then
                oDataMedium.FileName = oFolder & "\" & oFileName & ".pdf"
                oSTEPDoc.SaveAs(oFolder & "\" & oFileName & (".stp") , True)
                    
                Else
                    oDataMedium.FileName = oFolder & "\" & oFileName &  " Rev." & oRevNum & ".pdf"
                End If
                
                Call PDFAddIn.SaveCopyAs(oDrawDoc, oContext, oOptions, oDataMedium)
                oSTEPDoc.SaveAs(oFolder & "\" & oFileName & (".stp") , True)
                
                oDrawDoc.Close
                oRefDoc.Close
            On Error Goto 0
        End If
    Next
    '- - - - - - - - - - - - -
    
    '- - - - - - - - - - - - -Top Level Drawing - - - - - - - - - - - -
    Dim oAsmDrawingDoc As DrawingDocument
    oAsmDrawingDoc = ThisApplication.Documents.Open(ThisDoc.ChangeExtension(".idw"), True)
    oAsmDrawingName = Left(oAsmDrawingDoc.DisplayName, Len(oAsmDrawingDoc.DisplayName) -4)
    oAsmDrawingRev = oAsmDrawingDoc.PropertySets.Item("Inventor Summary Information").Item("Revision Number").Value
'
'    On Error Resume Next'    'Set the PDF target file name
                If oAsmDrawingRev = Nothing Then
                    oDataMedium.FileName = oFolder & "\" & oAsmDrawingName & ".pdf"
                    
                Else
                    oDataMedium.FileName = oFolder & "\" & oAsmDrawingName & " Rev." & oRevNum & ".pdf"
                    
                End If
                
        Call PDFAddIn.SaveCopyAs(oAsmDrawingDoc, oContext, oOptions, oDataMedium)
        oAsmDrawingDoc.Close
    
    MessageBox.Show("New Files Created in: " & vbLf & oFolder, "iLogic")
    Shell("explorer.exe " & oFolder,vbNormalFocus)
End Sub

Sub ConfigurePDFAddinSettings(ByRef PDFAddIn As TranslatorAddIn, ByRef oContext As TranslationContext, ByRef oOptions As NameValueMap, ByRef oDataMedium As DataMedium)

    oPath = ThisDoc.Path
    PDFAddIn = ThisApplication.ApplicationAddIns.ItemById("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}")
    oContext = ThisApplication.TransientObjects.CreateTranslationContext
    oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
        
    oOptions = ThisApplication.TransientObjects.CreateNameValueMap
    oOptions.Value("All_Color_AS_Black") = 1
    oOptions.Value("Remove_Line_Weights") = 0
    oOptions.Value("Vector_Resolution") = 400
    oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets
    oOptions.Value("Custom_Begin_Sheet") = 1
    oOptions.Value("Custom_End_Sheet") = 1

    oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
End Sub

[hamza_khan1]

Hi, i am trying to export Step files of the parts only from the main assembly and want the description and filename to be a part of Step file name. 

Is there any way around that? i tried to run the provided ilogic in sections but no result.

[SBix26]

I suspect that the Inventor Task Scheduler would be helpful here.  You don't say which version of Inventor you're using, but here is the 2020 Help section for Task Scheduler.

Task Scheduler allows you to select files to be exported by project, by folder, or by individual selection.  Hope that does what you need.

---

Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

[dliteful]

Hi hamza.khan -

I added a line to grab description from components and changed the Save As path (shown in bold green below).  This is more simplified than the PDF & STEP one that I posted earlier, but if you still want that functionality, just add to it.  Hope that's what you were looking for.

Sub Main()
	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
'	If MessageBox.Show ( _
'		"This will create a STP file for all of the asembly components that have drawings files." _
'		& vbLf & "This rule expects that the drawing file shares the same name and location as the component." _
'		& vbLf & " " _
'		& vbLf & "Are you sure you want to create STP Drawings for all of the assembly components?" _
'		& vbLf & "This could take a while.", "iLogic  - Batch Output STPs ",MessageBoxButtons.YesNo) = vbNo Then
'		
'		Exit Sub
'	End If
		
	Dim STEPTranslator As TranslatorAddIn
	Dim oContext As TranslationContext
	Dim oOptions As NameValueMap
	Dim oDataMedium As DataMedium
	
	Call ConfigureSTEPTranslatorSettings(STEPTranslator, oContext, oOptions, oDataMedium)
	
	oPath = ThisDoc.Path
	oFolder = oPath & "\_" & oAsmName & " STEP Files"
	
	If Not System.IO.Directory.Exists(oFolder) Then
		System.IO.Directory.CreateDirectory(oFolder)
	End If
	
	'- - - - - - - - - - - - -Component Drawings - - - - - - - - - - - -'
	'look at the files referenced by the assembly
	Dim oRefDoc As Document
	
	For Each oRefDoc In oAsmDoc.AllReferencedDocuments
		idwPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) - 3) & "idw"

		If(System.IO.File.Exists(idwPathName)) Then
			Dim oSTEPDoc As Document
			oSTEPDoc = ThisApplication.Documents.Open(oRefDoc.FullFileName, True)
			oFileName = Left(oRefDoc.DisplayName, Len(oRefDoc.DisplayName) -4)
			oDesc = oSTEPDoc.PropertySets.Item("Design Tracking Properties").Item("Description").Value

'
			On Error Resume Next
	'Save as STEP
	oSTEPDoc.SaveAs(oFolder & "\" & oFileName & " " & oDesc & (".stp") , True)

				
				Call STEPTranslator.SaveCopyAs(oSTEPDoc, oContext, oOptions, oDataMedium)
				oRefDoc.Close
			On Error GoTo 0
		End If
	Next
	
	MessageBox.Show("New Files Created in: " & vbLf & oFolder, "iLogic")
	Shell("explorer.exe " & oFolder,vbNormalFocus)
End Sub

Sub ConfigureSTEPTranslatorSettings(ByRef STEPTranslator As TranslatorAddIn, ByRef oContext As TranslationContext, ByRef oOptions As NameValueMap, ByRef oDataMedium As DataMedium)

	oPath = ThisDoc.Path
	oSTEPTranslator = ThisApplication.ApplicationAddIns.ItemById("{90AF7F40-0C01-11D5-8E83-0010B541CD80}")
	oContext = ThisApplication.TransientObjects.CreateTranslationContext
	oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
	oOptions = ThisApplication.TransientObjects.CreateNameValueMap
	
	If oSTEPTranslator.HasSaveCopyAsOptions(ThisApplication.ActiveDocument, oContext, oOptions) Then
    ' Set application protocol.
    ' 2 = AP 203 - Configuration Controlled Design
    ' 3 = AP 214 - Automotive Design
    oOptions.Value("ApplicationProtocolType") = 3
    ' Other options...
    'oOptions.Value("Author") = ""
    'oOptions.Value("Authorization") = ""
    'oOptions.Value("Description") = ""
    'oOptions.Value("Organization") = ""
    oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
'    Dim oData As DataMedium
    oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
    oDataMedium.FileName = ThisDoc.PathAndFileName(False) & ".stp"
oSTEPTranslator.SaveCopyAs(ThisApplication.ActiveDocument, oContext, oOptions, oDataMedium)
End If

	oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
End Sub