Computer Locking up longer than Feature Statistics rebuild time

[redbathtub]

Hello fellow Solidworks Users,

This week I have started a new job and have had the pleasure of working on an existing solid model. This model takes a ridiculously long time to rebuild initially. Then what will happen is when I edit a feature in the middle of the feature tree, Solidworks will become unresponsive and I'll wait. When Solidworks is finally responsive I can edit features/sketches slowly. Then when I check OK, it takes just as ridiculously long to rebuild. The Feature Statistics says it should take 68 seconds to rebuild when in actuality I'm waiting upwards (and in excess sometimes) of 10 minutes for solidworks to become responsive. This is obviously very aggravating and I appreciate if anybody is willing to help. My system specs are as follows:

Dell Precision T5500
Windows XP Pro 2002 SP3
Intel Xeon W5590 3.33 GHz
3.43 Gb RAM
NVIDIA Quadro FX 3800 (with the recommended drivers from the SW site)
Solidworks 2010 SP4

I have," Verification on Rebuild," unchecked and realview graphics off. I also have played with multicore support and hyperthreading with little improvement. The only thing I think may help is to upgrade to 64 bit to utilize more RAM. What do you think? Like I said, I appreciate your responses. I hope this is some option I am overlooking.

Have a great day!

-Andrew

 

[MadMango]

What type of features are you trying to modify? Anything in-context? Too many questions to ask in order to help, you need to give us a little more info. What is the long time drain in Feature Statistic? have you tried to recreate that geometry?

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[JMirisola]

As MM said, we need more info. What sort of model is it? How many, and what kind of, features are we talking about? Are you working locally or across a network? Do you have the 3GB switch activated?
If SolidWorks is crunching that long, it could be that there is some sort of circular reference that's causing it to bog down. If it's possible, post the model so we can test it out.

Jeff Mirisola, CSWP
Design Manager/Senior Designer
M9 Defense
My Blog

 

[redbathtub]

Mango & Jeff,

Thank you for the response. I'm trying to modify Cut-Extrudes, Boss-Extrudes, Fillets etc. The only contextural reference the part has is imported part geometries, the same part with multiple configurations imported multiple times. Could that be the hold up? The long time drain in the feature statistics is a Mirror feature. See attached .PDF of my feature statistics (I hope I uploaded it correctly). It's a large plastic injection molded part, about 24" X 24". I'm working locally. The part file is 117 MB, and IDK if my manager would appreciate me uploading our files to a public forum (this is my first week and all). I'll see what enabling the 3GB switch does. Thanks again!

-Andrew

 

[AnnaWood]

I suspect this part is very feature rich and what you are experiencing is a delay as SW updates the graphics area.

Two steps to a rebuild. The first is cpu based as SW crunches the numbers. Then your graphics card needs to crunch the data so it can show it to you on screen. For feature rich parts, with lots of faces, this can take some time.

Cheers,



Anna Wood
Core i7 EE965, FirePro V8700, 12 Gb RAM, OCZ Vertex 120 Gb SSD, Dell 3008WFP 30" Monitor
SW2010 SP2.1, Windows 7 x64

http://www.solidmuse.com

http://www.phxswug.com

 

[AnnaWood]

By the way, without actually seeing the part and being able to play with it, it is very hard to say what the issue would be and possible solutions.

You may want to call tech support at your VAR to get some help from them.

Anna Wood
Core i7 EE965, FirePro V8700, 12 Gb RAM, OCZ Vertex 120 Gb SSD, Dell 3008WFP 30" Monitor
SW2010 SP2.1, Windows 7 x64

http://www.solidmuse.com

http://www.phxswug.com

 

[CorBlimeyLimey]

If the file is 117MB you almost certainly will need more RAM.

Meanwhile, can you rollback the downstream features when working on the earlier features.

Also, suppress all patterns while editing.

 

[AnnaWood]

Suppressing patterns, fillets, any unneeded detail also helps in that it reduces the number of faces the gpu needs to process to refresh the graphics area.

More memory will not hurt. Unfortunately you will need to go to x64 bit to take advantage of it. I would have spec'ed your new workstation with Windows 7 x64 bit.

Cheers,

Anna Wood
Core i7 EE965, FirePro V8700, 12 Gb RAM, OCZ Vertex 120 Gb SSD, Dell 3008WFP 30" Monitor
SW2010 SP2.1, Windows 7 x64

http://www.solidmuse.com

http://www.phxswug.com

 

[redbathtub]

I appreciate the responses. The 3GB switch seems to have made no difference. Rolling back downstream features definitely helps as I realized this early in the process. I have also been combining as many features as possible which also helped. Perhaps I can convince my IT guy to upgrade me to 7. Thank you very much for the assistance. I guess I'll have to bring in a Magazine for when this model loads.

Have a great day!

-Andrew

 

[CorBlimeyLimey]

The /3GB switch will not dramatically increase performance, but should raise the bar to allow SW access to more RAM which in turn should allow more trouble free processing.

 

[JMirisola]

I'd be willing to bet it's the "... imported part geometries, the same part with multiple configurations imported multiple times..."
Configurations are nice, but, by definition, they're not the same part. While they, occasionally, have their place, I stay away from them as much as possible for production. I will admit that I use them more now that I'm in an R&D environment.
Depending on the nature of the references, SolidWorks could be trying to resolve more than just the part file you have open. Also, unless you're rolling back to the feature you're working on, any child feature would end up having to rebuild with each change. Obviously, once you roll to the end, they'd all update anyway...


Jeff Mirisola, CSWP
Design Manager/Senior Designer
M9 Defense
My Blog

 

[Updraft]

To follow the topic of parts with "in context relationships" as mentioned by MadMango. . .

If your part consists of features that are defined by relationships with other parts/assemblies then SWX has to check those during a rebuild. I have found this to be a big time sucker that doesn't get reported in feature statistics. This is especially true if your parts are all on a network. To see if this the case you should take a look at your features in the tree. If any of them have the "->" at the end of them then they have some kind of dependency on another file. If this is the case you should consider breaking these relationships and putting full control of the feature definition within your part. It will also speed up your part.

Using in-context relationships is a very handy way to develop part geometry, but our practice has been to break these relationships as soon as possible. Each part needs to stand on its own.

- - -Updraft