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)
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?
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?
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?
www.nxjournaling.com
RE: Save assembly to single file?
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?
RE: Save assembly to single file?
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?
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?
RE: Save assembly to single file?
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?
Older budweiser
NX8.5 & NX9.0 64bit, hp z820
RE: Save assembly to single file?
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?
www.nxjournaling.com
RE: Save assembly to single file?
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?
RE: Save assembly to single file?
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?
RE: Save assembly to single file?
I need a full assembly of flattened models (NOT A SINGLE FILE) somehow linked to the original models.
RE: Save assembly to single file?
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 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?
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?
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?
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?
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?
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?
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?
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?
No the customer is not expecting to get native files
RE: Save assembly to single file?
www.nxjournaling.com
RE: Save assembly to single file?
RE: Save assembly to single file?
www.nxjournaling.com
RE: Save assembly to single file?
RE: Save assembly to single file?
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?
“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV
RE: Save assembly to single file?
+++++++++++++++++++++
NX 8.0.3.4
RE: Save assembly to single file?
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?
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:
(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?
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?
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?
RE: Save assembly to single file?
www.nxjournaling.com