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]

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.

 

[skanskan]

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.

 

[cowski]

This sounds like a disaster in the making...

www.nxjournaling.com

 

[JohnRBaker]

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.

 

[skanskan]

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

 

[JohnRBaker]

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.

 

[RUGmechanic]

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

 

[SDETERS]

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.

 

[Toost]

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

 

[RUGmechanic]

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

 

[JohnRBaker]

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.

 

[cowski]

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

 

[JohnRBaker]

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.

 

[skanskan]

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

 

[cowski]

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

 

[Zarkomi]

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.

 

[busho]

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.

 

[JohnRBaker]

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.

 

[busho]

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.