How to create a lightweight faceted reference set

[cadmantools]

What is the procedure to create a lightweight faceted reference set to speed up the display process?

NX6.0.4.3 mp02, Windows XP 32-bit
Running cad straight out of the box is OK but, a system tuned with application software is the best way to increase productivity.

 

[daluigi]

Faceted representations was the earliest trick in the 3D CAD world to provide the user with less frustrations opportunities and it surely did its best within the '70s but I'm still very surprised that today's members still refer to that old dog as a solution more than an source of concern...

So why don't you look into using groups to filter out what you need to show at upper levels? That's so far the best thing I've found to be productive no matter what's been done before me.

 

[JohnRBaker]

So-called 'lightweight' representations are more critical now than ever. Besides, the use of 'facet' representations have become ubiquitous since if you're looking at a 3D shaded image, you're looking at what is basically a faceted representation, even if the edges and faces are considered to be precise.

Now in the way back past, those 70's daluigi was talking about, there were systems with represented that actual model as a faceted body and you're right, it did cause concern and was eventually replaced by exact or precise b-Reps, which is the absolute standard today, however, you've still got to generate facets to get 3D shaded images, just that it's now done as part of the display service and is hidden from the user.

But let's talk about assembly modeling where it's not necessary that all or even any of the bodies being displayed have to be represented as precise b-Reps. They can now be replaced by 'lightweight' (AKA 'faceted') representations and starting with NX 5.0, you can have a lightweight representation which provides you improved display performance and lower memory requirements yet when you need to reference the precise edge or face, that information can be accessed as needed, and this is being improved with each release, for example in NX 7.5 you can define assembly constraints between components which are lightweight representations. In fact, our longterm goal is to have the system work in a manner where the user NEVER has to concern himself with whether the model he sees is precise or lightweight.

Now getting back to the original question of how do you make sure that you're getting lightweight (faceted) Reference Sets. It's very easy. Just use NX as it came out-of-the-box, but to verify that those settings are still in place, go to...

Customer Defaults -> Assemblies -> Site Standards -> Reference Sets

...and just make sure that BOTH the Model and Lightweight Reference Set name fields are filled in.

In order to make sure that the system is loading the lightweight Reference Sets, you will also need to make sure that the Load Options have been set to prefer lightweight Reference Sets. Note that starting with NX 7.5 there will NO longer be any need for lightweight Reference Sets since the 'faceted' nature of the model is now part of it's definition and will be used whenever possible (although this behavior can be overridden, it our intention that it become the new normal way of working).

Anyway, I hope this answered your question as well as clear-up any confusion over when and where one would want to use 'lightweight' (AKA 'faceted') representations.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[daluigi]

[our longterm goal is to have the system work in a manner where the user NEVER has to concern himself with whether the model he sees is precise or lightweight]

That is the best piece of news ever, John!
That will for sure free the mind of large assemblies designers and allow them to finally display everything at the same time without having to built NX memory management strategies parallel to modeling/drafting - great!
Is that foreseen to be fully implemented into NX8?

 

[JohnRBaker]

NX 7.5 goes a long way to getting us to this state for Modeling, particularly when working with Assemblies.

As for Drafting, there's still more work to be done to fully leverage the lightweight representations but at least we're making it easier as Drafting is now smart enough to recognize that the Assembly model was using lightweight reps and so it will automatically replace them with b-Reps. So while we are still using heavyweight representations in Drafting, the user no longer has to worry about making the switch himself.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[cadmantools]

What do you do if you use wave linked features and need to edit the faceted reference set. Do I just remove the solid bodies of the component that I am linking?

NX6.0.4.3 mp02, Windows XP 32-bit
Running cad straight out of the box is OK but, a system tuned with application software is the best way to increase productivity.

 

[SiW979]

I appreciate the benefits of being able to work with superlite JT's etc, I can't wait to go to 7.5 especially considering the problems we have had with our large assemblies in the past, but one thing which continually vexes me is NX's inabilty to fully mate an assembly without doing lots of wave linking. Even if you do accept the fact that it is going to create a linked face (which we don't) it extracts he face minus all the detail in it. I'd love to see assembly constraints that work across the structure as well as just up and down the structure, it would make our lives a lot easier.

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX7.5 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[cyberpete]

John,

With an assembly of 30,000 parts (full vehicles) for interference checks, what memory savings would you see loading a full vehicle to see the faceted reps? That is a lot of memory usage for a lightwieght image.

Also, What happens to old style facets in assemblies? Is the legacy method supported or just dropped in 7.5?

 

[JohnRBaker]

I can't comment on your particular situation since there are so many variables involved. You just need to try different scenarios and standardize on those which prove acceptable.

As for what happens when you move to NX 7.5, first off, whether you use refile or not, when you open an assembly in NX 7.5 there will be NO faceted Reference Sets found in either the piece part files or being used in the Assembly. Faceted representation is now a characteristic of the solid/sheet body(s) which make up you model. They are there no matter what you do. Granted, you can ignore them and continue to use only precise representations in your assembly, but that will no longer be accomplished via Reference Sets, it will be an option, sort of like whether you wish to see your model shaded or not.

However, that being said, we highly recommend that you DO refile all of your files, including any reuse library/family table parts which are included in your assemblies since there is extra information which MUST be saved in your part file, not temporarily created on-the-fly when opening an older file in a new version of NX. This will be particularly critical if you are making drawings of your Assemblies and you have opted to use the 'Lightweight' mode when you're working with that assembly prior to creating or updating your drawing(s).

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[cyberpete]

John,

Thank you for your answer, but I need to separate in my mind Reference Sets and Facets.

If you could answer the following.

1. Do I have the option to use Assemblies/ Advanced / Representations in NX7.5 or is the function removed? If so, instead of saving to a reference set, will they save to a layer?

2. Will a part file created in NX6 with custom reference sets (ie: open) be unavailable to be toggled in 7.5?

Thanks

 

[cyberpete]

Bump - Need answer before Thursday 1 pm.

Anyone running 7.5 out there?

Thanks

 

[JohnRBaker]

In NX 7.5, unless you're creating a faceted representation of an ASSEMBLY, there is probably little need to ever use the Advanced options. If you are only talking about the lightweight representation used when a piece part (Component) is deplayed in an Assembly, Reference Sets NO longer play a role. The lightweight nature of the model is now a characteristic of the solid/sheet body itself. There is nothing there to place in a Reference Set nor find on a Layer. It would be like asking "on what layer do you store the COLOR of an object".

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

As for the second part of your question, YES in NX7.5, the NX 6 (and earlier) custom reference sets are still be available for use.

There is a customer default that allows these Reference Sets to be included or excluded (I assume that you want it included) from having lightweight data generated for the Reference Sets during refile or save. So, it will be possible to use the 'Open' reference set to control which body to use AND, if refiled in NX 7.5, it will be possible to choose to load that as lightweight or exact without having to use the representations dialog.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.