NX10 promote body
NX10 promote body
(OP)
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
What do you think?
I'm currently using NX10.
Thank you
Eric





RE: NX10 promote body
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.
RE: NX10 promote body
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
RE: NX10 promote body
www.nxjournaling.com
RE: NX10 promote body
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
RE: NX10 promote body
It's a used and required feature - which better be kept.
RE: NX10 promote body
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
RE: NX10 promote body
RE: NX10 promote body
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
RE: NX10 promote body
NX 9.0.3.4 mp12, TC 10.1
RE: NX10 promote body
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.
RE: NX10 promote body
Tim Flater
NX Designer
NX 9.0.2.5 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
RE: NX10 promote body
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.
RE: NX10 promote body
-Dave
NX 9, Teamcenter 10
RE: NX10 promote body
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
RE: NX10 promote body
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.
RE: NX10 promote body
Make sure you have your depth not set to through body.