NX 10 - Hidden bodies after STP conversion

[Bodnar]

Hello Guys!

I have a problem regarding displaying assemblies converted into the STEP files.

When I open the STEP file converted from the assembly (STEP214, by object selection) some bodies inside are hidden by default. This is somehow connected to the current reference set of the part. The problem exist only when I open the STEP file in NX - when I open this file in CATIA, every single body is visible by default. Any ideas how to manage that?

Thanks in advance!

Regards,
MB
M.Sc. Mechanical Engineering

 

[Toost]

From what system is the Step File ?
Where the bodies hidden there ?


Regards,
Tomas

 

[Bodnar]

Step file is made by NX10 software. Standard configuration, without any changes.

The hidden bodies are on the Part Navigator lists.

 

[Toost]

Are they hidden in NX when you export them ?

 

[Bodnar]

No, they are not hidden while exporting. They are hidden after I open the STEP file (in NX).

 

[Xwheelguy]

Just so we're clear, do you mean the bodies are not hidden in the ASSEMBLY NAVIGATOR (you state Part Navigator which indicates you're not exporting an assembly unless you're mis-typing Part Navigator rather than Assembly Navigator)? You should probably provide all the details you can about the Reference Sets being used in the source assembly as well as how you came to conclude that they're part of the issue when opening the STEP file.

What happens when you Import STEP 214 rather than use File -> Open? What are your Assembly Load Options set to (Search, As Saved, From Folder)?

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[Bodnar]

To make it completely clean: I export selected objects (by clicking on them) to the STEP file, they are not hidden while I'm selecting them.

- Indeed, sorry my mistake - the parts are not hidden in Assembly navigator (instead of Part Navigator).
- When I'm done with STEP transition, I open the STEP file once more in NX. Then in the Part Navigator there are some bodies hidden by default.
- The models are done by surface design and for the representation on the assemblies, I use reference set that contains only the last detailed solid body. Sometimes, when the model is easy, the representation could be 'Entire Part'.
- I see no difference between opening file by importing and opening (issue is still).
- The reference set was my first try, while I've pressed all parts into the final part reference set, then the STEP file did not contain hidden bodies by default.



Regards,
MB

M.Sc. Mechanical Engineering
Automotive Interior Designer
NX 10.0.2.6

 

[Xwheelguy]

So the issue becomes clearer now that all details are given.

Your surface bodies aren't going to automatically be added to the PART reference set (I think that's what you mean by "final part reference set") and in order for the translation to show those bodies (in NX at least) you're probably going to have to either add them in the source NX file OR after opening or importing the STEP change your reference set to Entire Part. Based on what you're describing, that's the way I'd test it out & see what happens.

Is there a reason why you're creating STEP files from NX and importing them back into NX? Other than checking the translation results (which as you have already seen isn't 100% accurate for checking how it will behave in other CAD softwares), that seems like a long way around opening an NX file directly or using a Parasolid export.

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[cowski]

To add to Tim's post, there are settings in NX that control what is automatically placed in the part's "model" reference set. The setting can be found in the customer defaults -> Assemblies -> site standards -> reference sets.

www.nxjournaling.com

 

[Xwheelguy]

Thanks for pointing that out, cowski.

Also, the PART (or "Model") Reference Set name can be named differently - ours (and I believe GM's) is set to be named PART. It's located in the same area that cowski pointed out.

To add to the Reference Set automation info we've already touched upon, you can choose to have both Sheets & Solids or only Solids automatically added to the "Model" Reference Set as well as setting nothing to be automatically added. I believe in the OPs case, both Sheets & Solids would be more appropriate for the STEP conversion to come back into NX as desired.

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M