NX UI

[sudhakarn]

Hi Folks,
I got a question here on the NX UI.I am from CATIA background.In CATIA the workbenches are grouped in such a way that the other modules cannot be accessed.But in NX,although we choose to open the model file,all the other modules like Assemblies,drafting and surface are also loaded.I want to understand if there is any speciality in it.
Also what is the meaning of display part in NX?

 

[NutAce]

Hi

I think the main reason for loading the other modules (although they are not all activated/active at the same time) is that you are able to switch between them fast.
Also, as of NX11, NX is able to switch automatically between them. It remembers in which module a part was last saved.

The Displayed part is mainly for Assemblies. You can show the complete structure on your display and ANT (Assembly Navigator Tree) while one of it's components is the Workpart.
The "Make Displayed Part" is removed as of NX12 and replaced by the "Open in Window" function.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[Toost]

NX works quite different to most cad systems regarding assemblies. I do not know how Catia works.
In NX the assembly file does not contain any geometry. Not until you possibly create wave link-s or Promote or create geometry there.
"Many other" cad systems will copy the geometry from the component into the assembly file, and keep an active link to the component file.
NX does not do that.
This means that when you have loaded an assembly, the geometry you see is the geometry that resides in the component file that is shown in the assembly file.
Thereby , if you want to modify that geometry, you need to make that file the work part, Or, the displayed part.
no matter which, the changes will be seen in the assembly file, without "update".

Regards,
Tomas

 

[sudhakarn]

Hi Nutace and Toost,
Thanks a lot for your insights.What i understand is that NX loads only a representation of the actual part file in the assembly.
Does the displayed part mean that its not the currently active part?
Please correct me if i am wrong.
Thanks a lot.

 

[Toost]

NX will load what you ask it to load.
The Load options has settings to control if you want to load all files fully or partially, or a lightweight representation (quicker), or not at all.
It is still using the same component file no matter how you load the component.
The assembly file is not modified due to how you load the components.

a few examples
If you work with say Plastic injection molds. You will do tons of geometric links (associative copying ) between the components, such that a change of the design automatically ripples through the entire assembly. Because of this, you will want to load all affected parts fully.
If you work with very large assemblies, say 100 000 components, you will want to load as lightweight as possible for performance. this is not the "fully load" option.
But when you select one of the components to modify, NX will automatically load that file fully . The others stay lightweight.
If you would open a large assembly but you know in advance that you only will work in a small area of that assy, you can load the assy "structure only" , Only the assembly file is opened, No components at all.
The assembly structure exists in the assembly file, you can there, in the assembly navigator, select the components you want to load and work with these. Leave the rest of the components unloaded.
what components are loaded and what components are not loaded does not modify the assembly file or structure.

The displayed part is the work part until you select some component and make that the work part.
Making some component the work part means "this is the file I will change and/or create new objects in".

imagine open an assembly. when done the assembly is the work part.
If you create a datum plane in this moment, it will be created in the work part, i.e in the assembly file.
If you make one of the components the work part and create a datumplane, you will still look at the assembly file but the datum plane will be written/saved in that component file.

Regards,
Tomas

 

[sudhakarn]

Hi Thomas,
That was a very detailed explanation.Thanks a lot.