convert multi body part into assembly 3

[SvenBom]

Is it possible to change a multi-body part into an assembly?
In solid edge, I can do it like this:
1. create a part with several bodies. Each body has its own name.
2. then I click on Multi-body publish command
3. in new window, I can see all the solid bodies, that will be saved into separate files. They all have the same folder destination as the original file. But, I can change those for each file. The names of new files are the same as the names of bodies in the file. I can also select Create Assembly command. With this, the assembly file with those bodies (new components) is automatically created.
4. click OK in this window and parts and assembly file are created.

I know, that in NX, I can use Create New Component. But, with this command, I have to create files/components one by one. I can not just click on a command and create all the bodies at once.
Is there any other way in NX to achive something similar to what I have described above?

Thanks for any info.
Regards.

 

[TheeCircle]

I could really use a how to on this as well!

Thanks in advance!

John

 

[JohnRBaker]

You could always write an NX Open program to do this.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[CAD2015]

"You could always write an NX Open program to do this."
How to do that, Mr. Baker? Can you provide us a step-by-step procedure?
I am very interested!
Thanks!


MZ7DYJ

 

[JohnRBaker]

Not ME! I don't write programs; I break them ;-)

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[CAD2015]

MZ7DYJ

 

[cowski]

Can you provide us a step-by-step procedure?

I'll take a stab at a rough overview:
[ul][li]install an integrated development environment (IDE) to use[/li]
[li]learn programming concepts: variables, branching, looping, arrays, etc[/li]
[li]get familiar with OOP and GUI design[/li]
[li]start a new project, reference the NX dll's as necessary[/li]
[li]record a journal using one or more NX commands you intend to use, clean up the resulting code and add it to your project[/li]
[li]remove the 'selection stickiness' from the journal code, add interactive selection routines as needed[/li]
[li]test your code with a simple use case[/li]
[li]fix logic problems and handle any errors that come up in testing[/li]
[li]add a GUI as necessary for users to interact with[/li]
[li]test the GUI, handle errors that occur[/li]
[li]imagine what can make your program error out, test those cases, add code to avoid or handle these errors[/li]
[li]add code to handle any unexpected errors[/li]
[li]give the code to John to break[/li]
[li]add code to avoid or handle errors, repeat[/li][/ul]

www.nxjournaling.com

 

[TheeCircle]

Can somebody show me how to do this within NX using basic commands?

LOL at Mr Baker!!!

Thanks in advance.

John

 

[CAD2015]

Thanks Cowski!

MZ7DYJ

 

[Tomerl]

If you do not need features information, you can export/import the file using Parasolid. it will create you dumb geometry in a correct assembly structure.
Writing code to do that is possible, though can be tricky if you have internal dependencies like expressions.

 

[TheeCircle]

Hi,

Sorry for sounding dumb but I have zero experience with journaling so is it possible to do this with NX component by component? Also adding the materials?

Thank you for everyone's patience with my lack of knowledge in NX.

John

 

[cowski]

Create component, basic overview:
[ul][li]Create or open a file that has one or more solid bodies in it.[/li]
[li]make sure the assemblies module is turned on (NX Start -> Assemblies is checked)[/li]
[li]Assemblies -> Components -> Create new component[/li]
[li]a 'new component file' dialog will open, enter a file name and save location for the new component[/li]
[li]the 'create new component' dialog will open, select one of the solid bodies, I suggest using the 'add defining objects' and 'delete original objects' options[/li]
[li]enter other options as desired, OK the dialog[/li]
[li]the solid body will be moved to the file you specified and added back to the original file as a component[/li]
[li]repeat for other solids that you want to convert to components[/li][/ul]

Consult the NX help file for additional explanation of the specific options.

www.nxjournaling.com

 

[JNieman]

I do exactly as Tomerl described.

It is common for clients to send us assemblies to modify or add to, but as multi-body .prt files. If we need to create assembly-cuts, additional component-level features, or exploded-view drawings to assist in shop communication, I will export the .prt to a parasolid file. Then I will import that .x_t file into a new .prt file made from the appropriate template.

It is a dirty way to do it as you now have two separate models to maintain. However, I know of no better way, and so far this has been relatively painless.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD LT, Autocad Plant 3D 2013, Enovia DMUv5

 

[SvenBom]

First, I would like to thank to all of you for your answers. Unfortunatelly, I don't write any programs, too. So, NX Open is not a real solution for me. It seems, that I will have to stick with more manual work, where an easy automated solution could be used. For big projcets, wouldn't this be an expected way of modeling:
1. create a layout with several bodies. Constraints and expressions can be used. But there is no detailing.
2. using Create New Component, each body is copied with WAVE linker to a separate file.
3. now, every department or engineer gets its own wave linked file and continue with detailing.
I guess I Will have to write to GTAC to open an IR/ER for this. And hopefully, NX20 will get this option, too.
Untill then, I will have to use other options and ways to deal with multi-body files.

As one engineer once said about NX:
The great thing about NX is, that it has so many options.
The bad thing about NX is, that it has so many options.

 

[schellenbergj]

And if you open an ER in GTAC you will get even more feateres in NX20

 

[cowski]

Extending the create component command to allow you to select and process multiple solid bodies in one fell swoop is a great idea. I encourage you to open an ER on the topic.

However, let's NOT add wave linking into the mix; the create component function works fine without it. Indiscriminate use of wave linking can lead to huge headaches (especially in native NX)!

www.nxjournaling.com

 

[SvenBom]

Why not using wave link?
Let's say, that there is a simple example like this:
1. open a new file.
2. create an extrude (simple block)
3. on top of this extrude,create second extrude. The first connection between those two is, that the second one is created on a top face of the first one. Then place some dimensions between the second extrude and the first one. Also create some geometric constraints.

Now, if I move those two bodies into new files/components with 'create new component' command, I will lose all the dimensions, created between bodies. I will also lose the geometric constraints, created between the bodies.

But, if I create new component with wave link, then I will keep the associativity to all the bodies and later I could make all the changes, that I need.

I have already reported this to GTAC under the IR1992829. I receieved an answer, that similar utility was already created by Mr. Jean Moreschi. He said, that I can publish his utility here on this forum, so I have attached the 7zip file. It contains the utility and the movie, that shows how to use it.

 

[TheeCircle]

SvenBom,

The file is asking for a password?

Thanks

John

 

[SvenBom]

Here it is without the password.
Sorry.

 

[Xwheelguy]

Granted, I only watched the movie....

Where is the option to name the components or is the journal using the feature names somehow? If the resulting component names aren't controlled in the top level assembly prior to running the journal, I'm going to have to rename 20-30 files every time I run this. I'd feel bad for anyone with more than 10 components. Nice of Siemens to pass along someone else's Journal, but where is the option for WAVE linking that some may want?

I'd call back and insist this be made into an ER to expand on what the Journal is doing and add more bells and whistles. Have WAVE linking be an OPTION the user controls with a checkbox - I really don't want to set a Customer Default and have to restart NX if this is ON (or OFF) by default.

Just my $0.02.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB