Step file that retains assembly

[will-eng]

I would like to create a step file of an assembly that when imported it comes in as a multi-level assembly. I have many parts broken out in the assembly that give description on what they are and intended uses. Currently when i import the step file in, it just comes in as a bunch of dumb bodies and loses the assembly structure.

When i import i make sure that the flatten assembly check box is not selected. I have imported step files from other companies that creates assembly components when i import it, so i know it is possible. Just wondering what i am doing wrong with either the export process or the import process.

Thanks for any insight into this.

 

[studiotreccani]

If you want to export the assembly with the tree you must select
the option "entire part", if you don't do that you will have
only a flatter part.

NX 7.5 64bit
NX 9.0.3.4 MP4 64bit
NX 10.0.3.5 MP3 64bit

http://www.studiotreccani.com

 

[will-eng]

When i do that it does not export anything. The step file is empty. What other settings do you have selected under the Advanced tab.

 

[Chaz4172]

Advanced tab, nested not basic?

 

[will-eng]

Chaz4172 Im not sure what you are asking. My basic setting are the same as shown in the screen shot posted by studiotraccani. I am wondering if it an additional setting that needs to be selected under the advanced tab on the export menu.

When i try to export entire part it doesnt export any data, the file turns out to be blank.

When i export selected bodies it flattens them into a single file and doesnt retain the assembly tree structure.

On the advanced tab ive tried selecting "export assembly as external reference", ive tried not selecting this, ive tried multiple combinations of these settings and either exporting entire part or selected bodies. Still no luck on getting the step file to retain the assembly tree information.

As for importing the step file i make sure that the flatten assembly option is not selected, so im not sure why it is not working.

I dont know if there is some other settings somewhere other than the export or import windows that i may need to change?

 

[Toost]

The line "selected bodies" should ring a bell i think. To me that will export the selected bodies without the structure.
Remember that in NX "a part" is not the same as "a single solid body".
NX has always had the ability to have multiple solid bodies and sheet bodies in one file.

Have you tried the option on the first tab "existing part" ?
have everything ticked on the data to export tab.
Then leave the Advanced tab as it was, i.e long names
color and layers , validation properties and export assembly as external references not ticked.

This should produce a "step assembly".

Regards,
Tomas

 

[will-eng]

Tried exporting "existing part" as well as exporting "entire part", and both yeild the same thing, and empty step file that is only 4Kb. No bodies in it no assembly structure. Thanks for the response Tomas but still not getting the program to export what it need.

Really makes me wonder if there is something wrong with the program. I've tried closing and reopening, as well as restarting everything.

Or again maybe there is more setting located in preferences or something.

 

[cowski]

If you open a piece part (not an assembly) and export a single body, does it export correctly?

Are you using the file -> export option from within NX or are you using the stand-alone exporter?

Edit: There should be a log file created during the export; open this file and look for "warning" or "error" messages for clues as to what is going wrong. Also, checking the NX log file itself may help (menu -> help -> log file, scroll to the bottom after attempting an export option).
www.nxjournaling.com

 

[will-eng]

File -> export. And if i have a single part open with multiple bodies in that part with no components it will export just fine.

But when i export a part that has no bodies in it, but has multiple subassemblies that have bodies inside of the sub assemblies. It does not export anything at all.

Unless i choose to export selected bodies and highlight everything. But then it is no longer a multi level assembly it just puts everything into one part and i lose all assembly information.

Update:
Checking the log file there are a few warnings but nothing that seem to affect everything exporting. The warnings say stuff like "! WARNING- solid body contains fault: 13805 - RTSTGX: Self-intersecting edge curve."

The only error read:
! ERROR- Failure code: 29
! ERROR- Routine: GTTGLI /
! ERROR- Message: invalid index

 

[PhoeNX]

I did some testing with an example assembly I have, which has no bodies in the assembly or sub assemblies, only the components contain a body.

If you export using Displayed Part, it will not create an assembly structure when imported.
If you export using Existing Part, it will create the assembly structure when imported, sub assemblies and all.

If you export with 'Export Assembly As External References' turned on, it will create separate files (either a STEP or NX part) for each component/assembly file.
Turned off if will export to a single STEP file.

The below image shows the settings I used to get a single step file as you would like (except for 'Export Assembly As External References' was turned off).

The attached STEP is the result of that export.



Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (29versions)

 

[will-eng]

PhoeNX

Thanks for the file i opened yours and it imports fine with the componenents ans sub assemblies all in there.

Tried doing what you said and i still get just a blank step file when i try to do step214. When i do step203 it doesnt even give me a file it has an error saying:

! ERROR- Invalid STEP file name.
! ERROR- File must have a '.step' or .stp' extension.
! ERROR- Unable to continue processing.

This made me think maybe my naming structure was causing problems but I tried creating a new assembly with a basic name, and imported your assembly into it then tried export your assembly into my own step file. Same problem. Either gives me a empty step file when exporting step214, or nothing cause of an error when trying step203.

Something is definitely wrong with the export. Just now how do i fix it.

 

[cowski]

Are you using "native" NX or do you use some sort of PDM/PLM (such as teamcenter)?
I ask because teamcenter often uses the "/" character (or is it "\"?) as the delimiter between the part number and revision. When NX tries to export 12345/A to a step file, bad things can happen.

www.nxjournaling.com

 

[will-eng]

no we do not use teamcenter or any file management system.

and the only special characters i use in some of the names are _ and -

but like i said i tried creating a assembly with a very basic name (model1) and used PhoeNX assembly that he was able to correctly export. And still was not able to get a file.

 

[PhoeNX]

Try the following.

File -> Open the step I uploaded (do not import into a new part file).
Once opened, it should be the correct assembly, with sub assemblies & components
Do a Save All, so all part files are saved.
File -> Export to Step (whichever format suits), but before changing any settings, click on the reset arrow (image below shows where on the dialog to click).

Then set for existing part, tick the boxes for all objects in Data to Export.
The resulting STEP file should be aroun 3Mb.


Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (29versions)

 

[will-eng]

Followed your exact instructions and came out with a step file that was only 30Kb, no where close to 3Mb.

Opening it up it looks like only the drawing border came through. No solids or sheets.

 

[PhoeNX]

What are your assembly load options set to (see image)?
It sounds to me like it's not able to load any of the components?

Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (29versions)

 

[will-eng]

The Assembly load options is set to "From Search Folders"

The folders chosen are structured like this "X:\CURRENT PROJECTS (NX)\..."

it has all of the folders necessary for all components to open. if the load options didnt the components would load into the assembly. So not sure why it would be able to see the components

 

[cowski]

From the pic above, it looks like your load options are set to "structure only" which means it won't load the component body data. Try changing the scope option to "all components".

www.nxjournaling.com

 

[will-eng]

Right after i posted the picture i went and tried just that and it worked.

Thanks everybody, really appreciate the time to help me figure this out.

 

[Rob_N]

From reading the 1st post, I was thinking something was wrong with you're load option settings.
Glad you got it sorted out.