Environment and file structure? 2

[cobaltred]

I have a couple of questions,Is there any difference between shape studio and modeling environment,it seems to me I can do everything in both environments?
The next question:I started a .prt file (modeling environment) or (shape studio environment) and made a base solid of let's say a computer mouse, I then created a feature group in the part navigator
and put all the features that created the base solid together.I then created another solid of one mouse button and did the same, created a feture group and put all that created the button together.
Now first, is this an assembly and a part and a drawing if I go into the drawing environment? and second, can I save out each feature group as an individual .prt file and then make an assembly from those parts?
Obviously I am a bit confused about what environment and file chioces to use, I thought everything in NX was simply a .prt file period, and you switch environments as needed.Any advise on this would be great,
I am not use to thinking about anything but a Solidworks workflow where everything is a part file or drawing file or an assembly file.

Last but not least, is history free mode used primarily for concept generation of base forms and can you get back your history if you switch from a histoy mode to a history free mode?

Thanks as always, Buddy

 

[SiW979]

Buddy

Firstly, there is no difference in any of the file types, be it done in modelling or shape studio or assembly or sheet metal. Basically shape studio gives you access to a few more specialist tools that are used for doing complex surfaces and surface editing. It allows Siemens to sell the product in modular form. So for me working in the excavator industry I would have no use for the ship building module. Somone working in a metal fabrication industry, would have no need for shape studio tools. For example, if you find the command called X Form or I form, then these are only available if you have the Shape Studio licence, there are a few other tools as well which can only be run on using that license, however, the part that is created will still be a .prt and can be opened by anyone with access to NX regardless of whether they have the correct licence or not.

In terms of your assemblies, then creating feature groups does not mean you are creating an assmebly. However the approach you describe sort of falls under the banner of what is known as Top Down Modelling. You can basically create all your solid geometry in one file then use the create new component option and select all the geometry you want to split out as a seperate component. When you do this, you will notice that the parts will start to populate the ANT (Assembly Navigator Tool) on the resource bar. Remember though! You must make sure that you select all and only the geometry that has been usd to create the solid for this to work. For example is you create 2 solid bodies by sketching on one single datum plane, then you will need to make sure that you have Delete Original Objects turned of, which will basically make a copy of the datum in to the new part.

Best regards

Simon NX7.5.4.4 MP5 - TC 8

http://www.jcb.com

 

[Toost]

A long question and a long answer
An assembly starts existing as soon as one adds a "component" to the part.
A component is "the object in the assembly that displays the other part at this location"

I.e create a new part, then either use "add component" or "create component", then this part has become an assembly. Delete that component and it is no longer an assembly.
( Similar to : "do I have any coins in my pocket , yes / no ?" )

A single part containing multiple bodies is not an assembly until one or more has been "converted" ( see Simons reply) into a component.

The so called Master Model principle, is in fact an assembly where the top assembly node contains the drawing, and normally only contains a single component, which in turn is the top assembly. But, NX allows one to create everything inside a single part if that would be desired.

The difference between shape studio and Modeling is as Simon says the license, and that the user interface is slightly different. The Shape studio UIF has been optimized for industrial design workflow, whilst modeling is "general use". All functions, such as X-Form and Extrude, are the same.


History free mode can be used anytime , I have yet not seen the true purpose/benefit since the history mode synchronous modeling is so smart done.
If the feature history is killed by switching to history free mode it is permanent.

Regards,
Tomas