Very slow assembly loading - NX5

[Simon205]

Hi,

A quick general question, that a search hasn't yielded any really relevant results for:

I'm working on an assembly with approx 30 components (mainly injection moulded plastic parts of reasonable complexity) and updating / saving the model is so slow (20+ mins) that I'm thinking that something must be set up seriously wrong.

Some of the components have wave-linked sketches between them, and now that the components have had radii added, it's impossible to save the main assembly (and some of the larger sub-assemblies) without 'out of memory' crashes.

System specs:
Dual Core AMD 4600+ processor
3.5Gb RAM
NX5.0.4.1

Any ideas appreciated,

Simon

 

[hudson888]

Are you working across a network. Generally networks are the culprits of first choice when thing are slow to load and save. Many users of NX are pretty dedicated to using that software for most of the time and don't necessarily always notice other network slowdown issues that may be in the background. If you're not working locally I would try saving a copy of the data onto the local drive in order to compare the loading speeds.

If it isn't that then have a look at the cue/status messages as the data loads and saves to see if you can spot a lot of updating going on. It may be the case that you have a great deal of wave linked geometry that is updating all the time and slowing you down. The recommended course of action would be to either switch off automatic updating and belay that until a time of your choosing or use the WAVE management tools to freeze some of the components.

Have you recently upgraded from an older to a newer version of NX? Many sites have systems whereby released data is write locked to prevent inadvertent changes and loss of design integrity. When you go up a version NX will on the fly upgrade your models from one to the other, so if you don't refile the data in the newer release then there may be a lot of updating going on and that could be the cause. The system will also warn you if it is unable to overwrite older files, so you ought to be able to diagnose this problem and hopefully refile to remedy the situation.

Teamcenter are you using it? Might it add to the list of possible factors? Wherever there is complexity the potential for something to slow you down usually exists.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[cowski]

If you are only interested in saving the assembly file, try using the 'save work part only' option (when the assembly of interest is the work part, of course).

 

[Simon205]

Thanks for the replies, in answer:

Yes we are working over a network - after your post Hudson, I copied the assembly and all parts to a local drive to test opening & update times and unfortunately noticed no real difference to working over the network. In fact, I get the same out of memory error crashes as when working over the network.

We don't have the Wave associativity manager, so are just using simple wave-linked references, and no, we're not using TeamCentre, and have been using this version of NX5 for about 6 months now (all parts definitely in NX5 format).

Thanks Cowski, but it's general updating & performance that I'd like to improve, as we're likely to need to come back to this model and make changes in the future.

I wouldn't have expected to have to uprade to XP64 and get more RAM for an assy with about 30 components, but perhaps this is the way to go?

 

[cowski]

Is is just one workstation that is the culprit or is performance slow on all of them?

Are you running certified hardware?

 

[Simon205]

There are 2 NX stations here, both running very similar spec, and at similar speeds (slow). I'm just checking the ATI site to see if there's a later driver for my graphics card (FireGL 5200) to see if this may be the culprit. Is there somewhere I can check to see what's NX certified?

For info, the parts within our assemblies are between 5-100MB each, with most being around 3-50MB, if this helps shed any light on the matter.

 

[cowski]

http://support.ugs.com/online_library/certification/

 

[Simon205]

Thanks, yep my graphics card driver is the one recommended, guess it's time to look into XP64...

 

[hudson888]

I guess that UGS can't test and recommend every available hardware configuration that is out there. Anything they reccommend will work and work well. I don't know if there are any indicators for relative performance, but what you have shouldn't be a bad card though and it appears that it is certified.

We have had some grief with high spec ATI cards before that were great for gaming but lousy for CAD. The deal was that they would sit and wait until the whole image was resolved before displaying anything keeping you sat in front of a blank window for quite a while before suddenly painting the entire image. We swapped them out for $250 Nvidia GeForce cards that weren't even on the certified list and came up trumps, with a 600% instant improvement. Because UGS don't test everything you often find that unless your needs are quite demanding the hardware that they test first and most often recommend is at the higher end and could be more expensive. Some hardware suppliers will allow you to swap out a few cards until you find the best one so long as you're able to travel to their store with your system.

We have also had grief with 64Bit OS and graphics drivers but only for NX-4, NX-3 and earlier versions of NX. I'm not seeing big performance deficits between NX-5 and say NX-3 on XP32 and nor do I think that the OS is likely to be the key performance factor in opening and saving files. This would be because a lot of it has to do with reading and writing from disk where you're hardware usually operates as the lowest common denominator over and above what the software influences.

If you are running any earlier versions of NX then perhaps you have similar data that you can open in either package to compare the performance. We have seen and heard of NO problems for people going from NX-3 or NX-4 to NX-5, but you never know until you rule everything out by testing it.

However If you have the files and system set up so that the files are being saved with a lightweight faceted reference set then you ought to be able to edit the default reference sets in your load options so that you hopefully achieve a noticeable improvement. That way if it really is the graphics performance at fault they you ought to be able to see some improvement and perhaps justify your worst suspicions.

If you're not working with faceted representations and need to know how then by all means post back but for the moment I'm suspecting that most experienced users are already using these tools to good advantage.

Do just confirm whether you're new to the system and whether you're working with legacy data from earlier versions of NX. I'd refer you again back to my earlier comments about refiling older data if that were the case.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Simon205]

Many thanks for the detailed reply and insight.

The graphics card thing is interesting, as my colleague's machine is running an old nVidia GeForce card which isn't supported and seems to run at a similar speed to my machine (with the ATI 5200), which leads me to thinking it may be a system setting thing or similar.

I've been using NX for about 8-9 months now (from SW) so yeah, fairly new I guess, but it's the updates that are killing us as it's gone from making a cup of tea and letting it update, to now having lunch. And no, there's no legacy data, these are all NX5 parts.

It's looking like getting 64 bit XP and loads of RAM at the moment.

Cheers,


Simon

 

[hudson888]

Simon,

You should probably try using Tools>Update>Delay Interpart.It works off the top pull down menus and when activated will have a tick alongside "Delay Interpart". For users without the advanced wave license you can avoid updating external wave linked geometry.

It isn't a sticky setting from one session to the next but can be activated under gateway before you load anything. If you decide you prefer it turned on permanently then you can edit the customer defaults to do so.

If this isn't you problem then I'm unsure what is? Perhaps we should hark back to lightweight geometry. Using lightweight geometry doesn't just relate to graphics performance, it also saves memory.

By the way all indications are that your graphics cards are probably okay based on what you've told us thus far.

If you're using XP/32Bit with 4Gb or ram then do try turning on the /3Gb switch to optimise your memory performance. If you google XP 3Gb switch you should find ample explanations about how to go about that.

Also set your maximum and minimum virtual memory paging file sizes to the same maximum size I have them at 4092/4092. If you have less that 4Gb of RAM on a 32bit system running NX-5 then larger models will slow you down quite easily.

I have one similar system that is still capable of opening up very large assemblies with minimal fuss under NX-5 with relative ease, so I suspect whatever is wrong in your case ought to be fixable!

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum