One of my customers has sent me a STEP file they are having problems with when importing in to Inventor 2014.
When they import it, it imports successfully as Inventor ipt and iam files but the browser (node) names are llisted as the component descriptive names, but when you interrogate the file names in the iProperties they are listed as part1, part2 etc. which is not very helpful.
I have imported the same STEP file into Inventor 2013, and the behaviour is as expected i.e. the bowser names match the files names (i.e. they are the descriptive names, not part1, part2 etc.)
I have tried all the different import settings in the dialog box, but can't seem to resolve it.
Any help would be appreciated.
When you export a STP, the part names in the assembly's browser (ocurrences) will be the same when you import the resultant step, also the part's "file names" will maintain. But it's possible to have a diferent "assembly's browser part name" and "file names" for the same part.
I think maybe... when you export the STP, maybe you change the name in the assembly browser, but forget to change the file names, can be possible?
Since Inventor 2014 uses new data translation platform, so there is behavior change compared with legacy (Inventor 2013).
For the instance name, Inventor 2013 gets produce name as its instance name while Inventor 2014 gets NAUO name as instance name and will rename instance name only if there is duplicate one.
For the solid body name, Inventor 2013 gets name from SHAPE_REPRESENTATION in the STEP file, if string is empty, using part name as body name. Inventor 2014 gets name from MANIFOLD_SOLID_BREP or BREP_WITH_VOIDS, if string is empty, use inventor default, such as "Solid1, Solid2,...".
To do a further investigation, can you share your STEP file here or via email Hongyuan.Li@autodesk.com and attach some images to show the problem ?
I thought more and did more investigation and understood more about your problem, the problem I suppose is the instance name is not equal the document name, take below structure for example:
When open the Instance1 or Instance2 in a new document, the document name is shown part1 or part2 in Inventor2014, so when you save it on the local disk, the file is part1.ipt or part2.ipt, seems this naming conversion is not very meaningful because it just use the default Inventor naming rule. Let me give more explanation:
Behavior change for document/file name:
Please open your STEP file with Notepad++ and find keypoint string "PRODUCT", take below code for example
code format is Product ('ID', 'NAME', 'DESCRIPTION'), so in this example, ID=1332_010_002_000, NAME=N/A, DESCRIPTION=N/A
In Inventor 2013 the code logic is to use string of PRODUCT-ID as its document/file name, and let instance name = document/file name. In Inventor 2014 since we changed the legacy behavior since we think it is more make sense according to STEP specification that use PRODUCT-NAME instead of PRODUCT-ID as document/file name, but in this case, the PRODUCT-NAME string = N/A, so we will follow the Inventor default naming rule which use part1, part2, ......partn as its document/file name.
Behavior change for instance name:
Please open your STEP file with Notepad++ and find keypoint string NEXT_ASSEMBLY_USAGE_OCCURANCE, take below code for example:
code format is NEXT_ASSEMBLY_USAGE_OCCURRENCE('ID', 'NAME', 'DESCRIPTION')
In Inventor 2013 we set instance name = document/file name which use PRODUCT-ID. In Inventor 2014, we use string of NEXT_ASSEMBLY_USAGE_OCCURRENCE-NAME as its instance name, if no NEXT_ASSEMBLY_USAGE_OCCURRENCE defined in the STEP file, we uses Inventor 2014's document/file name as its instance name which use PRODUCT-NAME. If the NEXT_ASSEMBLY_USAGE_OCCURRENCE-NAME is N/A, we also will follow Inventor default rule which uses part1, part2, ......partn as its instance name which seems not very meaningful. But I think we do the right thing based on STEP specification because we should use string of PRODUCT-NAME or NEXT_ASSEMBLY_USAGE_OCCURRENCE-NAME instead of its ID to shown in the browser.
I will collect this case in our customer feedback pool and discuss more for this behavior change if more and more customer reports got for this change.
thank you for your suggestions, I'm not sure exactly what I am looking for, as I couldn't find any lines that said N/A. So I have emailed you the STEP file directly, if you can take a look and let me know what you think.
Apparently another STEP file import worked fine with the bowser nodes matching the file names, so it would be interesting to know what is causing it in this case.
As a temporary work around we have imported it into 2013, and then opened and saved in 2014, not ideal but a fix for now.
We have a customer who is very angry with this change. It's not acceptable. Can you add an option (registry key by example) in roder to use the old STEP import?
Thanks for share the customer feedback in the forum!
We are taking a look it now.
You can refer to the above temporarily workaround that is imported it into 2013, and then opened and saved in 2014, you can also email the STEP file to me Hongyuan.Li@autodesk.com I will double check and update the STEP file to match Inventor 2013 behavior.
Thanks for this proposition but it's not an isolate case. This customer need to import STEP weekly. But can you develop a tools to clean the STEP file in order to open it in 2014 like the 2013?
Thnaks in advance.
Thanks for feedback and understand your requirement.
We are now discussing this internally and will update you the result as soon as possible.