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Save assembly to single file?
5

Save assembly to single file?

Save assembly to single file?

(OP)
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)

RE: Save assembly to single file?

Well you can have two DIFFERENT files, one a "functional assembly" and one that is just a bunch of solidbodies. Now that second file, the one which has been 'flattened' into a single file, will no longer update, unless you take some extraordinary steps, when any of the Component files update like what happens in the "functional assembly".

To get this 'flattened' Assembly file, open your Assembly and go to...

File -> Export -> Part...

...and specify a new file name, change the 'Object Selection Scope' to 'All Objects' just in case there are sub-assemblies, select 'Class Selection' and pick all the Solid Bodies (and Sheet Bodies if that's relevant). Now if you are only interested in just the dumb bodies and NOT all the features and expressions, select the 'Remove Parameters' option and hit OK. Now you have a copy of your assembly only it consists of a bunch of bodies, arranged propertly, all in a single file, but no longer linked to the original Assembly or its Components.

Now if you DO want this new 'flattened' file to somehow remain linked to some extent with the original Assembly and its Components I can give you some ideas as what some of the alternatives are, but I'll wait for the response before I waste a lot of electrons explaining it.

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.

RE: Save assembly to single file?

(OP)
Yes it would be nice.

And what about wave linking all the parts or
there also was a command to "move" the part to the assembly level.

RE: Save assembly to single file?

This sounds like a disaster in the making...

www.nxjournaling.com

RE: Save assembly to single file?

Why do you want this 'flattened' assembly in the first place? What is it going to be used for?

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.

RE: Save assembly to single file?

(OP)
Just for curiosity and because it's easier not to get messed with many files.

RE: Save assembly to single file?

I would squash your 'curiosity' ASAP. You do NOT want to consider this as if it were a viable workflow. It's NOT!!! And trust me, I will NOT be the last person to tell you 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.

RE: Save assembly to single file?

Maybe closing in to a disaster, but...:

Would saving your assembly into a single part file (containing only dumb solids and sheets) be an easy way to save the current "state" of the assembly ?
It's like making a screenshot to show how the design evolved over time or how many alternative designs there were over time ?
Like day 1: assembly_dump_1.prt, day 2: assembly_dump_2.prt, etc...

I know, NX is not ment to be "dumb", so is there a better, more "sophisticated" way of saving alternative designs ? Or maybe a rule of thumb or sound engineering practice?

Older budweiser
NX8.5 & NX9.0 64bit, hp z820

RE: Save assembly to single file?

Could you just save different Revisions of the assembly? Are using teamcenter? So each day you save a new revision of the assembly and then lock it down so it can not change.

RE: Save assembly to single file?

If you use Teamcenter, there is a "snapshot" option ( do not ask me where or how) which will save the assembly and all components as it looks at this very moment.
i.e similar to "Like day 1: assembly_dump_1.prt, day 2: assembly_dump_2.prt, etc... "
Note though that you need lots of disk space since each snapshot is a complete copy.


Regards,
Tomas

RE: Save assembly to single file?

I don't use Teamcenter. To me it seems that creating a dumb copy isn't a bad idea after all, considering disk space. Or am I missing some clever NX tool?

Older budweiser
NX8.5 & NX9.0 64bit, hp z820

RE: Save assembly to single file?

If you're talking about a so-called 'flattened' Assembly with all the bodies, dumb or otherwies, in a single file, you may not be saving as much space as you think. With a 'normal' Assembly the Assembly files only contains the structure and constraints but not the Bodies or topology of the components. In many situations, the Assembly file is rather small when sitting the disk. Granted, when you open an assembly all of the component data has to be loaded as well into memory, but even then NX only loads what's absolutely necessary for working in an Assembly. For instance, all of the feature data is left behind, until a Component is made the Work Part, and now with Lightweight Representations we don't even have to load all the solid topology just to get something that you can see when looking at the assembly as a whole. Also, if everything was all in one file, ALL of the data would have to moved from the disk, which might actually be a server on network, and loaded into memory everytime that 'flattened' Assembly was opened. Whereas with a noraml Assembly you can set it up so that you can load only the Components of interest, leaving most of the data back on disk. This really can make it efficient to open and work on something if you don't need it all at once. With a 'flattened' Assembly, it's ALL or nothing. And the same thing happens when it's time to save your changes. With a normal Assembly, when you hit Save the only files that are written back to disk, which could be on some network server, are the main Assembly and ONLY those Components that have been modified during your session, which could anywhere from NONE to all, but most of the time only a very few. You don't have that with a 'flattened' Assembly, again when you hit the Save button you have send the ENTIRE part file back to disk on waht could be a network server.

No, there are very good reasons why we designed Assemblies to use the 'referenced' data structure and not to have to load everything into the same file all the time. Also, when it comes to reuse common parts, you don't have mess with Assemblies files just to find where the actual data is or have to make sure which is the latest and where it might be located.

And besides, are you really going to compromise the performance and usability of your Product data models all for the sake of avoiding having to buy a few extra gigabits of disk space?

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.

RE: Save assembly to single file?

If you want to save snapshots of your assembly (native NX), you should look at the clone function. If you want them for archiving purposes, you should search for "UGZip" in this forum. Someone made a utility that essentially copies your assembly to a zip file.

www.nxjournaling.com

RE: Save assembly to single file?

Here's a link to the Eng-Tips forum where the 'UGZip' utility was discussed and from where you can download copies of it.

http://www.eng-tips.com/viewthread.cfm?qid=345894

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.

RE: Save assembly to single file?

(OP)
Does the receiver of the ugzipped file also need to have UGZip installed on his computer?

RE: Save assembly to single file?

Quote (skanskan)

Does the receiver of the ugzipped file also need to have UGZip installed on his computer?

No, the result of the UGZip program is a compressed (.zip) file containing the assembly file and all the components. The person receiving the zip file only needs a way to un-zip the file, which is pretty much built into the OS these days, and the proper version of NX to work with the files. When they open the assembly, they can use the "as saved" or "from folder" load option, either should work.

www.nxjournaling.com

RE: Save assembly to single file?

How to do opposite way from flatten file to assembly with individual part files. When the file come from application with all in one structure. Visi, keycreator etc.

RE: Save assembly to single file?

JohnRBaker explained the process of "flattening" perfectly, but how to do that with some kind of links to the original models?
I need a full assembly of flattened models (NOT A SINGLE FILE) somehow linked to the original models.

RE: Save assembly to single file?

When you say 'flattened' are you talking about an Assembly with NO Sub-Assemblies, as in a single-level Assembly, that is ALL the Components in the top-level Assembly itself? If not, could you try and explain it again?

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.

RE: Save assembly to single file?

Ideally I would like to get a product tree with the assembly consisting one level of parts. The parts should have the geometry removed and be linked to native files with geometry. What's important, the result should be the assembly file and part files as a separate entities not just one merged file.
If that is problematic or not possible I need to find a way how to remove geometry from a single part files maintaining somehow a link to a native files. That actually would be good enough and it would serve it's purpose.

RE: Save assembly to single file?

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.

RE: Save assembly to single file?

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.

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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.

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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.

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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

RE: Save assembly to single file?

The customer is not as responsive as you guys:)

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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.

RE: Save assembly to single file?

Quote (cnc07)

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:

Quote (busho)

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

RE: Save assembly to single file?

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

RE: Save assembly to single file?

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

RE: Save assembly to single file?

(OP)
I've opened the Pandora's box, jeje

RE: Save assembly to single file?

I think Pandora's box was a computer...

www.nxjournaling.com

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