NX10 promote body

[Eric Ferland]

Hi, I just have been told by our NX support team that building assemblies using the promote body function (for fabricated/machined parts) is not a clean way to do it.

What do you think?

I'm currently using NX10.

Thank you

Eric

 

[Javiduc]

Hello Eric,

I also use promote body for machined parts and I have been told that this command may be deleted from future NX releases which scared me a lot because others ways to represent machined assemblies are worst thant promote body.

I think promote body is a bit buggy command. For example, if you use them for assemblies inside assemblies in several levels like some times I have to do; sections in 3D do not show section lines, some times when editing a sketch I can't see the promoted part, some times exporting to step It exports both the original part and the geometry with machined features... and thinks like that.

But this command is needed for machined assemblies in order to have the components parts without machining and also the assembly with the machined features. Without promote body you have to use wavelinking I think, but it is more strange because then you have the geometry twice in the assembly which is very strange way to do it and may lead to mistakes (other softwares doesn't need to do that in this strange way you directly make features to the components without any need to promote or link).

One thing that I like about promote body is that you can bend or make other sheet metal features to a part after welding which is not very common but sometimes needed and there is not other way to do it.

What I think NX need is a better way to do what promote body does. I don't know if by improving promote body command or by creating a good new way to do what promote body does (not by wave linking and duplicating geometry) A direct way to make threaded holes or chamfers to several componentes with just one feature (like assembly cut). Fix bugs like the ones I told before... and keep the way to bend a component inside an assembly.

 

[3dr]

Not only does "Promote Body" eliminate the duplicates in your assembly, but Promoted Bodies also respect parts lists and ballooning in drafting.

It would be a big loss if this functionality was lost.
It's the only real tool NX has to "design as you would build" in assemblies.
Welded assemblies & Cast parts are perfect for this tool.

Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1

 

[cowski]

The notion that "promote body" is going to be removed has been floating around for years. The last "official" announcement on the topic stated that promote isn't going away. Not only is it a useful command in itself, but it is also used internally to other commands (such as assembly cut and hole series).

www.nxjournaling.com

 

[Toost]

I agree with Cowski. If Siemens does something, i rather suspect them to upgrade the architecture behind the promote feature.
It's also used in the NX CAE when one wants to simplify the model for calculations.

Javiduc: Logically a promoted body is also a duplicated body as a Wave linked body is, but the interaction is simpler on the Promote body.
The big question to me is why there is no "hide parent permanent" in the wave link.

Regards,
Tomas

 

[Yevgeny N.Yurovitsky]

"Promote" allows you to design the very same way you manufacture.
It's a used and required feature - which better be kept.

 

[JohnRBaker]

When WAVE linking was introduced, the Promote architecture WAS updated shortly after that to leverage some of the work that was done for the WAVE project, without of course losing any of the unique behavior of Promoting versus WAVE linking.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[Javiduc]

Hello John, thanks for the info. If promote architecture had improvements, then I guess that the information I got about this command going to be erased is not correct.

 

[JohnRBaker]

That is correct, there are no plans to discontinue support for Promotions (at least when I left the company in January).

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[cmacca]

Would be great if you could relink a promote if it breaks it's link. Currently the only options are to recreate which can be very complicated if the promotion goes multi level, or convert to a wave link which has the draw backs mentioned above

NX 9.0.3.4 mp12, TC 10.1

 

[Javiduc]

I totally agree. Promote body is a great command, much better than wavelinking, but needs some improvements.

Not as useful as relink, but I think it would be good if the command let users to define in just one step that all components of an assembly should be promoted and united and even better if this is done with other components added afterwards automatically(maybe it is a bit more difficult). I sometimes have holes applied to some promoted bodies (I have just learn that unite them help me to work with them) but then I modify my assembly and I have to promote new components and apply the holes to that bodies.

 

[Xwheelguy]

Enhancement Requests logged with GTAC would get the ball rolling for those seeking improvements.

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

 

[Javiduc]

Hello Xwheelguy, thank you for your advise. Yes, I will probably place an ER for promote body (and for other improvements too), It will take me some weeks though. I have been learning NX for a few months and we have recently started to use it in the company, we had a "trial" period and now we have just received the final licenses so I think we are able to place ER now. I think I still need to learn more about the command before that, for example I wasn't using "unite" after "promote" and this took me a lot of unnecesary repeated hole features that I don't need now (I still think that hole feature should let you go through more than one body, though). I want to be sure that what I am asking for, is really needed and that is the best solution I can find, and also a realistic request. Posting here and reading other people post helps me a lot with that.

Promote body is in my oppinion a very good, and powerful command (Is a better way to do the job than the one for other softwares I have seen, and better thank wave linking because os geometric duplication, part list...) but I think it need some improvements. For the kind of products we design is not useful but mandatory to use this promote body, its because of that that I was so worried about it.

Now, I think the way "unite" command works for promoted body can be improved in some ways, for example when you select a component in the assembly navigator if that component have been promoted and united to other you don't see this component selected in the graphic window and I think it would be good. I have also seen some extrange behaviors (promoted bodies I can't see when editing a feature applied to this bodies...) but they don't always happen so I need to learn more about them.

 

[Dave K]

A few years ago, I submitted ER 6982977, looking for the ability to convert a wave body to a promoted body. You can go the other direction, but occasionally we had users that just wave linked, not knowing about promote. I thought I included the request to relink promoted bodies, but it appears not.

-Dave

NX 9, Teamcenter 10

 

[cowski]

I still think that hole feature should let you go through more than one body, though

If you use the "hole series" option within the hole command, it will let you select multiple bodies from different components to create the hole. Let's say that you want to bolt three components together and you want to add the hole at the assembly level; the "hole series" will allow you to select the three bodies and make a clearance hole in the first two and a threaded hole in the end body all within the same command.

www.nxjournaling.com

 

[Javiduc]

Hello cowski,

With hole series I can't make a threaded hole to different bodies, I mean with threads in different bodies. I need to create threaded and not threaded holes through different components (all different components have to have threads if the hole is threaded or not threads if the hole is not threaded) and store the hole geometry at assembly level, not at component level because those holes are machined after welding.

 

[SDETERS]

You can set the Boolean in the thread hole command to none. Then use assembly cut and/or subtract with hide tool body turned off to create the thread hole in the multiple bodies.
Make sure you have your depth not set to through body.