UG NX v7.5.2.5 Update Display Unresponsive Graphics Broken 1

[mag00n]

First Here are the specs on the system;

Alienware Area51 ALX

Intel i7 990x @ 3.46GHz
12gb DDR3 Ram
Dual 1.5GB NVIDIA GeForce GTX 580 w/SLI
Windows 7 Ultimate x64

We have two of these systems that were ordered and shipped at the same time.
They are both running UG NX 7.5.2.5
Both have the latest graphics drivers, and SLI is disabled on both.
Whoever is reading this should assume that all the nVIDIA graphics settings are the same on both. Also, the settings for "Visualization Preferences" inside UG are the same.

The issue I am having is when working in Modeling inside an Assembly the graphics on one of the systems is showing broken lines and instead of smooth circles, multiple straight lines are displayed.
When this happens on system "A" (the good one) the user can RMB (Right mouse button) and select "Update Display" and everything refreshes to show true radii and smooth edges.

System "B" (the problematic one) will not do this. Upon clicking on Update Display the screen doesn't respond as if its not initiating the command - whereas with system A, when you click the same command the model disappears for a split second and refreshes with perfect lines/arcs/edges.

I DO NOT believe this is a problem with the graphics card(s) for many reasons.

If I make a part that is showing broken lines and edges in the assembly my displayed part, clicking on "Update Display" works like it is supposed to. If I make that same component my work part while still in the assembly, it automatically shows that same bad surface as a smooth perfect edge. Although as soon as I make the assembly my work part again, the edge reverts to its broken form.

If I open an assembly I have previously created using NX6.3 it displays great using that version! Not a single graphics issue using the problematic system. But if I open it using version 7.5.2.5, any 3D edge containing a radius looks broken until selected individually from the assembly.

I have attached a screenshot from the problematic system that shows how bad the edges of a curved surface display.

I believe this is a simple setting either somewhere within the customer defaults, or in a menu I have overlooked a thousand times.

I have already wasted half a day on the phone with GTAC ticking and un-ticking settings in my nVidia settings and a few others inside UG with no change. I am also aware that these graphics cards are not on the "Supported Cards" list. But since 6 of our other systems are running dual GeForce cards and one of them is an exact duplicate of the problematic one, I don't believe that is the issue. GTAC was stumped and reverted to the standard "If its not supported and the three things we tried didn't work, your SOL" *No real complaints about GTAC support, until this issue they have been awesome and I encourage everyone to use their services.

Hopefully someone out there has run into this issue, or at least heard about it and can offer a solution or an idea to work with.

Thanks!

 

[cowski]

Disclaimer: If GTAC was unable to help you, it is unlikely that anyone on this forum will be able to do better.

With that said, you might want to try an older graphic card driver. Sometimes the newest one presents new problems.

 

[JohnRBaker]

While I no idea what might be causing the differences between your two systems, as for what you're calling 'bad edges', since you say this only happens when you're looking at the parts of an Assembly this is probably due to the fact that you're looking at the Assembly with the Components loaded as Lightweight Representations (AKA Faceted bodies). When the Assembly is the Work Part, the Components are displayed as lightweight, but when you change one of the Componets are displayed as precise, which IS the as designed and intended behavior. The difference between NX 6.0 and NX 7.5 is that in NX 6.0 you had to explicitly set-up Assembly Load Options to use the Lightweight Reference Sets when open the Assembly to see anything like this. However, in NX 7.5 there are NO Lightweight Reference Sets anymore and the system can now display Lightweight Representations as just a normal display of the Solid/Sheet bodies of ANY Reference Set. So now you can leave the Components as Model Reference Sets and let the system determine automatically when and if the system needs to use the Lightweight or the Precise models when working with an Assembly. This being done to provide the maximum level of graphics performance without the user having to constantly decide when and if the Components are loaded Lightweight or not. In other words, what you're seeing is what you should be seeing. It's by design!

Now you can disable this behavior but it's an all or nothing setting now since there is no way for some components to be loaded lightweight and others not. If you wish to NOT see the lightweight representations when you open your assemblies, go to Assembly Load Options and you will see an option in the 'Scope' section of the dialog named 'Use Lightweight Representations'. If you toggle this OFF, then when you open your assembly all the Components will be loaded as precise representations. However, you display will take longer to load and changing views or rotating your display dynamically will not be as fast or smooth. Therefore we recommend that leave the Assembly Load Options as they are and simple learn to use the system as it was designed. If you do you will get better load times and faster display response while working in the context of the Assembly. The system will automatically load precise date when and if you need it so there is generally no need to ever worry abour switching Reference Sets or changing load options using the new scheme as it will now be taken care of for you as you change tasks and set Components to be the work part or not.

Anyway, I hope this helps. As for the differences that you're seeing between your systems, make sure that when you're running NX that the Assembly Load Options have been set the same on both systems.

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.com/museum/

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

 

[mag00n]

That worked! Un-ticking 'use lightweight representations' did the trick. Strange that the tech on the phone didn't have me try that..

Right after I changed that setting I tested the loading and displaying of one of the larger assemblies in our library (over 400MB total) with no noticeable difference in load/display time.

I can only verify that on this system which has some pretty hefty hardware.

I can say that this is a must if any design house uses screen sharing meeting software for design reviews! Its really hard to explain why components look like they are crashing when they really aren't to a customer who isn't familiar with UG!

Thank you for your advice John, your a life saver!