Export of Creo part is successful but is devoid of any geometry

[tbraxton]

I have a part model that is solid geometry. When exporting the part using STEP it generates the file but the STEP file does not contain any geometry when imported.

The part does not have any geometry checks and has absolute accuracy (1E-4 inches) set in Creo 7.07. The geometry is not what I would call complex.

I have been able to get around this issue by saving the part as a Creo neutral file, opening it as a part and then exporting it as STEP. This process yields accurate geometry in the STEP export.

The source part file will not export to STL either but there is no diagnostic info on bad geometry. Typically this would identify are where tessellation failed.

Has anyone else encountered this issue?

[remy]

Creo opens empty when opening the STEP export of the above part. It is surprising indeed as the geometry is mainly prismatic.

Can you clarify the below:

1. what protocol do you export to?
2. is the STEP file of size 0 ko?
3. what does the content look like when you edit the step file with notepad?
4. by change have you ever tried STEP Analyzer? STEP File Analyzer and Viewer | NIST it is an agnostic STEP tool used as a controling tool.
5. when importing the STEP file, do you include a template? if yes have you tried without it?

[Patriot_1776]

Weird.  Is it a file created in Creo, or is it imported?  Does it give you a mass when you do a mass properties?  If it's an imported file, and you have Solidworks, import it into that, "fix" it there, and export it as a STEP.  I'm guessing here because I'm stuck on Creo 4....until I switch to Creo 8 in the next couple weeks.

[tbraxton]

The part file is native Creo geometry created in Creo 7, it does use a copy geom driven by an external reference.

The Creo part reports accurate mass when measured in part mode.

I have tried the following STEP protocols exporting solid geometry only.

ap203 is

ap214

ap242

STEP file sizes are not=0 but are small i.e. 14Kb & 250 lines

Warning message upon opening STEP file in Creo as a part:

Could not construct feature geometry.

[Patriot_1776]

The copy geom may be screwing things up.  Can you delete it or suppress it before making a STEP, or does the Creo geometry reference the copy geom and will fail if you do either?

[tbraxton]

The copy geom is the first feature in the model of with geometry, it is a parent to all solid geometry in the model. It looks like I will need to open a support call.

[kdirth]

Differences in model accuracy between the model and the inherited model have caused issues for me in the past.

[tbraxton]

All absolute accuracy values are the same among all of the parts as they should be in this context.

[tbraxton · Accepted solution]

I had an external vendor test this part for export and they got the same error as I did in a different environment and without any input from me other than to save it to a STEP file.

I have finally found the root cause (operator error). I was using a STEP profile that excluded construction bodies. This is a feature of multi body functionality introduced in Creo 7. 

In some circumstances Creo will convert a body to a construction body without user input. That is what happened here. I was excluding construction bodies from the STEP export.

When replaying the model the only body in the part is changed to a construction body when an external copy geom feature is added to the model. This happens with no message on the command line or other notice. I found it by adding body display to the model tree and watching the icon change indicating the switch to a construction body. You can only observe this with the body icon expanded.

[Dale_Rosema]

WOW! Good to know for future use.

[mneumueller]

Please note that the ECG has settings within its option panel to control the propagation of parameters.

This includes several aspects ranging from appearances to body names and more, and it also includes an option to propagate the construction body attribute. It also depends on whether an external body/or bodies are added "as is" or being merged into the existing body in the part.

Here is how the options look like:

Hope that helps

[tbraxton]

@mneumueller 

Is the setting Construction yes/no a logical  toggle when redefining the ECG feature in the target part? I tried editing the definition of the ECG and unselecting the Construction yes/no. When I regenerate the body is still a construction body. I must be missing something and I cannot find details of this in the on line help files.

Thx

[mneumueller]

yes, it is a logical toggle that allows to control whether the status/attribute from the source should be propagated to the target.

If you "uncheck" it, the "construction" body attribute/status will no longer be propagated to the target. That means an update of the ECG will no longer force an update of the construction attribute in the target body. In your case, I assume that means the target body will stay a construction body (simply because that is its current state  and no update is forcing the body to change that status.) If you do a right-menu action on the body to "Unset construction body" status, then the body should become a regular solid body and should no longer change to construction during an ECG update.

[tbraxton]

@mneumueller 

Thanks for clarifying this, it resolved the issue for me.

I was able to activate the toggle option in the ECG and then manually unset as construction on the body to establish the design intent for the part as desired. Unless I missed something in the on line documentation, I think more detail should be provided for this in the help files. There are some nuances of multibody that most users will never figure out without some more explicit documentation.

Your on line multibody tips are useful and appreciated. I miss the old style user manuals which were much more comprehensive than the current on line docs in most cases. I still have a set of physical books from Pro/E release 17 on the shelf that I sometimes still refer to.

[Patriot_1776]

'Sup Tom!

Wow, ok, good to know, thanks!  I would say that if it's doing that WITHOUT USER INPUT, that that's a bad thing.  But of course, PTC will call it an "Enhancement!", RIGHT?  LOL

I'm going to (have to) transition to 8 soon, so, good to know all these "New And Improved!" bugs...  😉

[RonanM]

I had the same issue with a native single body part, I have an empty STEP file while my body is not a construction body.

I've changed the part accuracy and the STEP output format without sucess.

Nevertheless, I've found an indirect way to export it : copy and paste the body to create a new one. The 2 bodies are exported in the STEP. file The first remains empty while the second body is correct. 

[mneumueller]

Hi Ronan,

that sounds like a somewhat different problem. 
I think it would be great if you could report that to Technical Support, so it could be understood.

Thank you very much.