Save assembly to single file? 5

[skanskan]

Hello.

I've seen assemblies that are completly contained in a single prt file.
How can I save my multipart assemblies to single ones? (And still having a functional assembly)

 

[JohnRBaker]

So you're saying that you would like to basically remove the hierarchy structure of sub-Assemblies and move all the Components up to the top-level assembly. That way you will only have to deal with ONE Assembly file, which references the actual part model files, and the part model files themselves but nothing else, correct?

Now are we talking about you already having Assemblies which have extensive hierarchical structures, i.e. several level deep sub-Assemblies? And you want to 'flatten' these existing Assemblies, correct? In other words, you're NOT creating any NEW Assemblies, just restructuring one or more existing Assemblies, correct?

Are you looking for a description of an interactive workflow to do this or are you looking for some sort of utility or custom program that you would execute to do this automatically? IKeep in mind that if you've only got a few Assemblies to flatten, getting someone to write a custom program for you may not be all that productive.

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.

 

[busho]

It might be that I understand the concept of top assembly a little bit different as I've got my experience only from Catia V5. I have attached the screen shoot of an example of my product tree. It might tell you more than words.
I would like to remove all geometry used to create sub assembly files, but without moving them up in Assembly in any way. So the assembly structure will stay the same (with multiple children under one parent assembly file as on attached screen shot) only all those sub assemblies are going to be "flattened" to a dumb solid bodies, but still linked somehow to the original files with full geometry so if I would modify the originals, the dumb solid file would update automatically.
And again, if for example the sub assembly is build with 2 extrudes, I can't have them extrudes merged into one solid, I need 2 solids, obviously without sketch used to create it.
But as I said previously, opening a single file (not a whole assembly) and saving it as a dumb solid with multiple solid bodies would do the job if I could still have a link to the original file with geometry somehow. It would be good enough because I would still be able to create Assembly with these dumb sub assy files.
And again the crucial thing is to have all sub assemblies as a separate .prt files not one.

 

[helperug]

as far as a I understand not a allcatpart.
try this :
open each the sub assembly in new window, wave link all assembly member body into assembly level. From assembly navigator switch the members to reference set empty.


sorry new in NX
regards
Erwin

 

[JohnRBaker]

May I ask WHY IN THE WORLD ARE YOU LOOKING TO WORK IN THIS MANNER?

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.

 

[cowski]

Since you are coming from a different CAD system, let's take a step back and describe how NX handles parts and assemblies. What you are describing sounds to me like basic NX assembly functionality.

Some CAD systems have multiple file types depending on the contents (model, drawing, assembly, etc); NX has only the one type (.prt files). An NX .prt file can be a model, drawing, or assembly. An assembly file contains links to the individual model files, but does not contain their geometry. In the model file you can create "reference sets" which define what geometry you want to see in the assembly; in this way you can filter out items such as datums, sketches, etc etc. When a part is added to an assembly, you can specify which reference set to use initially and of course, this can be changed later within the assembly. Every part will automatically have an 'entire part' and 'empty' reference set, and the out of the box (OOTB) default is to also create a reference set named "MODEL" that will automatically contain all the solid bodies (and optionally all the sheet bodies - zero thickness surfaces that do not enclose a volume). If the model file(s) and assembly file are open in the same session, any changes made to the models will automatically be shown in the assembly. A model file can be edited in the context of the assembly by making it the 'work part' (right click the component and choose 'make work part'). When a component is made the work part, all the defining geometry is loaded into memory (if it is not already) so that you may edit the defining features.

There are a few ways to create your assembly file, the most common work flows are called 'bottom up' and 'top down'. For illustration, let's say you are modeling a toy car. In the bottom up work flow, you would create a 'chassis.prt', 'wheel.prt', 'axle.prt', and 'body.prt'; then you would create a 'car.prt' and add the other files as components positioning them and/or constraining them as necessary. In the top down work flow, you would create the 'car.prt' and start modeling the other parts as solid bodies within this file. At such time in development that you decide you want a proper assembly, you can use the NX assembly function 'create component'. Using this function, you can select a solid body (or bodies) and NX will export the body and defining geometry to a new .prt file and add it as a component back to the car.prt file. Now you have all the defining geometry in its own file and a component (or link) to that geometry in the assembly file.

From your description it sounds like you started with the top down approach and are now looking for the way to create components. Make sure the 'assemblies' module is running then use the command finder to search for 'create component' to find the menu location. And of course, look up 'create component' in the help files for more information on its use.

www.nxjournaling.com

 

[busho]

Thanks Cowski for your description of NX functionality, I'm sure it will be helpful to me sooner or later but I'm afraid that it's not going to help me with my task.
Our customer requested models only with solid bodies but also with some kind of link to our models with full geometry. It also might be beneficial for our company to not to send them editable models. I assume that if I would sort that with reference sets the customer could still get access to our geometry within the models.

 

[cowski]

Does your customer use NX? Are they expecting to receive native files? If so, you may want to ask them for clarification of what they want exactly.

In a few posts you mention: "models only with solid bodies but also with some kind of link to our models with full geometry", which sounds like a basic NX assembly (the components are links back to the original geometry); but you also mention: "...if I would modify the originals, the dumb solid file would update automatically". I know of no way in NX to output dumb bodies that update when the originals are edited - this is a contradiction in terms. Dumb bodies are not associative to anything, hence the term "dumb".

www.nxjournaling.com

 

[busho]

Well. Theoretically these dumb solid files would update only if they are loaded to NX together with a native files. This is how it works in Catia V5. You can do "copy" and "paste special with a link". The result of that is a dumb solid but only if you don't have a native file open in the same time. Therefore for the customer it is just a dumb file but for me it is a file linked to native file which allows me to update the dumb solid instead of creating it again. I'm pretty sure there must be a way of doing it in NX
No the customer is not expecting to get native files

 

[cowski]

If your customer is getting files in a neutral format (parasolid, step, iges, etc), then it doesn't matter so much what you do in NX. There is no option to associate these types of files to the original geometry. Each time your model or assembly changes, simply export a new copy and send it to your customer.

www.nxjournaling.com

 

[busho]

Well. They still require .prt files, but for some reason they don't want to see the construction geometry of the model.

 

[cowski]

You sound quite confused as to what your customer wants. For you own sake, sit down with the customer and ask a lot of questions as to exactly what they want. Better to ask an 'obvious' question now than to deliver an unusable mess.

www.nxjournaling.com

 

[busho]

The customer is not as responsive as you guys

 

[cowski]

Well, for what it is worth...
If someone gave me a packet of work and instructed me that they "don't want to see the construction geometry", I'd take that to mean that there was nothing modeled in the assembly file (no extraneous solids, sheets, curves, etc - only components) and the components used reference sets to filter out the part level construction geometry. Furthermore, in the part files I'd move the finished solid body to layer 1 and move the construction geometry to other layers and turn those off. If/when the part file is opened, the model is there to inspect without the clutter of the other geometry, but the geometry is there for when edits are necessary.

As an NX user, this makes the most sense to me, but again - you'll have to verify with your customer.

www.nxjournaling.com

 

[ewh]

I agree with cowski. If that is not an option, I think helperug is on the right track. Just wave link all of the components into your assy file and replace their reference sets with "empty". This will help to maintain the associativity on your end, allowing you to keep control of the component parts if you send the customer only the assembly file. When they open it, the links will be broken and they will in effect have dumb solids.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[Mechman50]

Wouldn't an Engine Assembly be a good candidate for this flattening. I don't make the engine; it is a STP file supplied by Kubota. After importing the STP file, I end up with 300 individual parts to this assembly. I will never be changing the design of this engine, I just would like one single file representing this engine.


+++++++++++++++++++++
NX 8.0.3.4

 

[cnc07]

helperug and ewh explained it correctly for what busho asked.

I see that using wave links is the way to go in this case regardless your customers have the same CAD system or not for the native format be it Catia or UG or anything else.
1. It protects your IP
2. And the files' sizes are much smaller.

 

[cowski]

helperug and ewh explained it correctly for what busho asked.

You may be right. Wave linking the geometry then breaking the links would essentially give you "associative dumb bodies"; however, I don't think it will satisfy this requirement:

I would like to remove all geometry used to create sub assembly files, but without moving them up in Assembly in any way.

(emphasis mine)

I'd argue that wave linking the body into the assembly moves it "up the assembly".

www.nxjournaling.com

 

[ewh]

Good point...
You could wave-link at the component level and use the wave linked files in the assemblies, in effect creating two files for each part. Instead of moving the parent components "up" in the assy, it would move them "down".

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[looslib]

Mechman, yes it would and that is what we used to do at a prior company. The engine supplier would send us their engine assembly file with all components in the structure. We would export and import through STEP to get a single part file of the engine blob. All we needed were the mounting block surfaces to position the engine in the machne.
One thing we did was keep each engine in a separate directory since we used multiple models and some with the same component part numbers. In the official CAD folders we only kept the blob part.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[skanskan]

I've opened the Pandora's box, jeje