Solidworks CANNOT cope???

I work at a place where we often works in assemblies with 5000+ components, 1500+ sub-asemblies etc and its seriously getting on my tits the amount of times solidowrks crashes/freezes each day.

My desktop is a Dell Precision Intel Core 2 duo @ 2.66 Ghz with 6GB RAM and an Invidia Quadro FX4600 (768mb) graphics card.

Surely companies which design heavy industry stuff, like aerospace, oil & gas or whatever must use larger assemblies than we do, how do they manage?

Is my PC up to the job?..what else can we do to get a more stable system?

Thanks

Those industries probably use other software, like CATIA, Pro/E that seem to be meant for “heavier lifting”

I’ve understood solidworks as the entry to mid-level design package.

The PC should be up for it, unless it’s always crawling along sluggish-slow.

Are you running XP64 or just regular XP professional? If you’re not in 64 bit then you’re limiting yourself to 3 gigs of available application RAM regardless of how much you have in the machine.

Most of the times people working with assemblies that large are only viewing a portion of the data or simplified versions of the data at one time.

Realistically though, crashing tends to just be a fact of life sometimes, esp when you push the system hard. Even on HP workstation which is a vendor certified dual-Quad core machine (8x2.66) with 16 gigs of ram and a 1.5 gig Quadro 4800, I get more than my share of crashes from Pro E or Alias.

I’m not fluent in working with Solidworks, so I’m not sure if its a stability issue with your machine, or a limitation of the software itself.

If you aren’t tied to Solidworks then perhaps it’s worth talking to other vendors about some of the bigger systems like Pro, Catia or Unigraphics.

In addition to above suggestions, I assume that you are running lightweight for the parts or sub-assemblies not needed at that time? In addition, I am also assuming that you have automatic rebuild suspended?

We find that working in lightweight or large assembly mode can cause problems in that some information gets missed from the drawing, such as decals, which we need to show. So we have to work in standard mode. Generally, working on the model is fine and does not behave sluggishly, but it does crash alot. And yes, we are running x64 but im not sure solidworks is using all available memory, how can you check this?

Thanks

you should talk to your VAR and complain. I bet they try to get you to upgrade to Catia! I spoke to some NASA folks last month with the same problem. They quit trying to push solidworks and instead went back to Pro/E. Its a good thing because all the solidworks users who refused to use proe got the pink slip. Buck the system and you get bucked

You really need to get in touch with your VAR. The hardware you are running should be doing the job and by your own admission your models are not sluggish but crash a lot. This could be down to a couple of things;

1.) Was antivirus off when Solidworks was installed and when service packs updated?
2.) Is ypur graphics card driver up to date? This can be checked at solidworks.com
3.) Are you on the latest service pack?

I am applications engineer for Cadtek a UK solidworks reseller and it is difficult for us to help customers who dont let us know when they are having problems. We wouldn’t try sell Catia and dont sell Catia and as your are modeling in the thousands this is within Solidworks’s capabilities.

Taking DesignEngines advice and moving to ProE is not guaranteed to fix the problem. I also think he should make it clear that his company specializes in ProE training, so he is going to be bias and he does comment on Solidworks posts suggesting moving to ProE.

Get in touch with your VAR and let them try help.

I did not suggest to go to proe.

A friend of mine is a solidworks advocate and pushed to get NASA to use Solidworks on a project. When solidworks choked on the big assemblies they were forced to go back to Pro/E (like everyone else at NASA)

Method:

Some considerations for working with Large Assemblies…

  1. Though Lightweight mode was already suggested, it should at least be noted that it is subjective to what you have going on. So if the component that has the decal is needed then leave that “Fully Resolved”, and leave the rest in LIghtweight.

  2. Speed Pack: Speek Pack allows you to tell the program what parts/bodies/surfaces you want loaded when you bring in that Sub-Assembly into the Top Level.

  3. Configuration: I don’t care if you have a Cray Supercomputer or IBM Blue Gene…you put 10,000 blots in a model with the threading on each (and the threading was done with a helix and sweep) there is going to be a hit in performance. Hell you can hardly get humans to multi-task past 3 things at once and be cognitive…:slight_smile: With this in mind being mindful of how things were modeled. Can there be a simplified version of that model. If you look at the “Feature Statics” of your Part Files or Assembly Stats, this can be a good way to begin to gauge where and why the program is taking a hit.

  4. Top Down Assembly modeling: Some go this route, others stay clear of it. Everything in moderation right…so if there are hundreds of Part files with a ton of “External References” if/where you can, break them. Skeleton modeling or Layout modeling is often one key way to have a master Assembly model that is completely Locked but is shared with all team members. This way everyone works from the same page, but are free to work on their respective areas.

  5. Working across the network: Avoid at all cost. Just asking for trouble even with gig switches, routers, NIC cards. Always work local and use the built in Data Management System to move the files from local to network drive.

Hopefully these are at least some starting point to take a look at.

Pieces…

You should look into Autodesk Inventors capabilities around large assembly managment. Check out Rob Cohee’s video on YouTube addressing large Assemblies: http://tinyurl.com/mhg8cz. -Best, Jamie Gilchrist