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Light version of assembly

Pioneer
Pioneer

Hi people, can you tell me is it possible to save an assembly which have many parts and it is hard for manipulation as a part, strictly part (or parasolid) without bodies as a components? If is possible I would like to get my assembly just like a shell. Every other version is hard for me.

5 REPLIES

Re: Light version of assembly

Siemens Phenom Siemens Phenom
Siemens Phenom

Hello IloveAudi86,

 

I wouldn't advise to save the assembly without the components.

 

If you load an assembly, you can easily just load the structure of it with a setting in the Assembly Load Options (See picture below)

2018-01-23 15_51_28-.png

 

There you can set the Scope --> Load --> Structure only (see picture below)

2018-01-23 15_50_26-Assembly Load Options.png

 

When the assembly loaded, you can only see the structure and load the parts you want to see by just setting the checkmark (see picture below)

2018-01-23 16_16_32-NX 12 CAM_nx1202 Build CAM_nx1202.89 - Manufacturing.pngs

 

If you wanted something else, please let me know.

 

Cheers

Alexander

 

Re: Light version of assembly

Genius
Genius

Have a look at NXs Bookmarking functionality. 

 

One thing is to decide what to load in which way (see Assembly Load Options). The next question is whether you want do make the same decisions (what to load how) again and again. Bookmarking should allow you to store the information what you have loaded in what way (lightweight, not at all or else) for your next NX session.

Best wishes,
Joachim

In production NX 12.0.1.7 D2
In testing NX 12.0.1.7 MP4

Re: Light version of assembly

Pioneer
Pioneer

Thank you Alexander, but that is not a solution for my problem, because your path don`t release assembly from unnesessary bodies. Anyway, I am thankfull for this detailed desription of path.

Re: Light version of assembly

Pioneer
Pioneer

Thank you J.S. but I still wonder how to avoid chosing what to load and when as you mentioned. there is obviously no way to aplicate my idea.

Re: Light version of assembly

Genius
Genius
Without knowing your assembly situation it is difficult to give advice.

What you immediately should do is use the Assembly Load Option called Partial Loading. I am at home now and don‘t have access to NX. The NX online help does not specify its name correctly. Partial loading component parts does the following: Instead of loading the BREP (boundary representation) + design features (history) of each component of your assembly it loads the BREP only. That should save you 20-30% of memory. Also, if you set the proper ReferenceSet in each component part (you have to do this in each part of your component), you can specify which body/wireframe to load and display when using partial loading. All bodies/wireframes not being in the used reference set are not loaded into memory. When you enter a part of your assembly it gets automatically loaded into memory with its feature history.
Depending on what you set in your workpiece (part, blank, check geometry) you could omit loading certain components at all.
You could also WAVE link the part geometry you need to your CAM part and not load the component part at all (like Andreas mentioned before loading structure only)
Because setting this up or optimizing what you actually load and display, the bookmarking functionality can help you restore this loading state in a later NX session.

As a final optimization topic you could use is the Simplify Assembly command. But it creates a simplified representation of your assembly which means a facet body. I don‘t know if this is really what you want.
Another command would be Wrap Assembly, but I assume the result is too coarse. Without NX at hand I cannot tell you anything about its parametrization.

I would propose the following:
Part: For part geometry load the BREP of the geometry on which you actually have to program your machining on.
Blank: If you really have to use it with a large assembly, then use a facet body representation.
Check: In the worst case use only the bodies of parts that is really giving you a risk of running into. I once had a user selecting every screw below the machining body and performance was really poor.

Generally, you can find some stuff in the NX online help section about Large Assemblies.

As I wrote it really depends on your parts and what you do.

I hope I have not messed anything up due to my long writing.
Best wishes,
Joachim

In production NX 12.0.1.7 D2
In testing NX 12.0.1.7 MP4

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