How to avoid - rendering invisible lines- UG Drafting Module 2

[Rhyder88]

I am supposed to create a drawing with large assemblies. Even if i am using light weight representation, it is taking very large time to create the drawing view and badly ending with memory insufficient error.

I observed that it is taking too much time in the step"Rendering invisible lines" . When i tried to create the view without "hidden line processing" the views are created within seconds eventhough the data is large.

Is there any settings to be changed to avoid this issue. My requirement is "Creating drawing view with large assemblies as light weight representing data and hidden lines should be processed . Without hidden line processing the views look very confusing because of too much lines

 

[JohnRBaker]

What version of NX are you running?

John R. Baker, P.E.
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[Rhyder88]

version is 7.5

 

[JohnRBaker]

If you're running NX 7.5, even if you've created an assembly using Lightweight Representations, when you make a Drawing of that Assembly the Lightweight Representations of the Assembly Components are automatically replaced with Exact Representations.

Now this does not mean that you have no choices but if your desire is to add dimensions and labels to your models, create section views, use anything other than fullly-hidden line views, etc., then you really have NO choice but to use Exact Representations. Now if all your you're looking for are non-dimensional, non-sectionable, fully-hidden line views no your drawing you can use 'Faceted Represetnation' views, which will be very fast, but they will also be tessellated (i.e. faceted) which may or may not be acceptable, but it will be fast.

There are some additional things that you can do in NX 7.5 to speed things up, such as extracted edges, but that will only work with Exact Representations so you have to at least spend the time to properly create an exact view which can then be converted to simple curve which will then allow the Assembly to be unloaded leaving just the extracted curves behind, which you can dimension and add labels to with no problems, however if changes are made to the models, then you will need to perform at least one full update for every model change, but until you need to load the models so that views can be updated, performance will be better than if you had not extracted the edge curves.

That being said, starting with NX 8.5 (which is already available for customer downloading and production use) the system WILL be able to use those same 'Lightweight Representations' tha you built your Assembly with, in your Drawings, EVEN if you NEED to create dimensions and notes attached to the model, create section views or even have something other than a fully-hidden line view (such as dashed hidden lines). While these NX 8.5 Lightweight Representations will NOT be as fast as the pure 'Faceted Representations' available in NX 7.5, they will be significantly faster, and use less memory than if you had used Exact Representations for your Drawing views. In fact, you should be able to simply default to using 'Lightweight Representations' for most all cases where you have to create drawings of complex part models or large Assemblies.

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.

 

[Rhyder88]

Thank you very much John. Meantime i explored with some options. I Enabled the option File->Utilities->Custom default->Assembly->Site Standards->Facet reperesntation->"Load smart weight Data" . I just want to know whether this option increase / decrease the performance of software.

In addition, i have a doubt how HIdden Line Processing affect the speed. HLP in the sense, the software will not categorize any line as hidden line. Every line will be visible in even width. The performance varies when HLP is on/off.

 

[JohnRBaker]

Note that toggling ON the 'Loading Smart Lightweight Data' option does result in a bit more memory being used and thus may have a slight impact on overall performance when opening a large assembly, however, if you're going to do alot of in-context modeling or editing, this will actually improve your overall productivity since more tasks will be able to be performed immediately using the 'Smart Lightweight' data already loaded without having to stop and load additional exact data.

Hidden Line Processing is, by definition, a compute intensive operation (the good news is that this task does lend itself to muti-threading therefore the Parasolid kernel is engineered to take advantage of muti-core processors when computing hidden lines). This is an area which is constantly being worked-on and we've taken additional efforts with the new NX 8.5 use of lightweight representations in Drawings to get the most out of methods for computing and displaying hidden line rendered Drawing views.

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.

 

[Rhyder88]

Yes John, as you said i experienced performance variation when 'Loading Smart Lightweight Data' is toggled on.

Now i used to create a view by Create base view ->Right click on screen->view style->Base->Toggle on 'Facet Representation' option.
and General->Extracted Edges -->None
Now the view is created pretty fast.But the problem is HLP computation doesn't takes place.

I dont know how to overcome this. Now whether i need to change any visualization settings or some-other settings?

Note:I dont need to give any dimensions or sections or annotations in the view. Just i need to show an exploded view of a large assembly. And i need to update it often. But i also doubt that updating the view is possible or not because i set Extracted edges as None.