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New to Solidworks

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ten4jdf

ten4jdf

Mechanical
Mar 5, 2009
5
I have used Solidworks for a few years now but never full time because of the lack of speed. We are now trying to go full time on this but once again the speed is an issue. We do machinal design with large assembly that average 4000 parts. Modeling seems to be okay but doing the assemblies and especially drawings is were we see problems. Are there any suggestions on how to deal with this?
 
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What are your full system specs?

Which SW version and SP?

There have been major advances in both system and SW speed over the last 'few years'.

A 4000 part assy isn't that big. Are you using individual sheet or multi-sheet drawings?
 
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4,000 part assemblies are not THAT cumbersome with the right hardware, drivers, and modeling discipline. Can you tell us the version of SolidWorks and the hardware specifications of the workstations you are using? Some indication of the types of assemblies could prove useful as well.

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

Have you read faq731-376 to make the best use of these Forums?
 
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Stay away from v2008. In theory, you can make use of the SpeedPak feature in v2009, but it takes some set-up time, and you shouldn't modify/tweak things in those paks without being fairly careful everything updates properly. Otherwise, those ought to be useful for critical attachment points or other faces within the assembly to optimize performance.

The other solution is to move to a 64-bit OS like Vista. Believe it or not, people have had good success running SW within Vista 64.



Jeff Mowry
A people who value security over freedom will soon find they have neither.
 
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okay guys, i have never used a forum before so taking me time to figure this out.

I have a a Dell Dual Core 2.66ghz. w/3.25gig ram and a Nvidia quadro FX 3450 video driver running solidworks 2009.

As far as what type assemblies????

what we have done is develop our main bodies in a part. This part has three solid bodies in it with one of the bodies being subtracted (indent) to form a cavity in the other two. this is then put into an assembly and then the other parts are added to it. most of these parts are our standard parts already modeled and are on a seperate server. the assembly and main bodies are on our local drive. As i understand it, working across the network can be a problem.
 
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oh yeah, my IT guy has a 64 bit machine that isn't being used (to many conflicts when used before) so we are going to try it later today. We run autocad too so we hope there aren't any conflicts running both on this machine.
 
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Are you even using all your RAM currently? If so, do a search for "/3GB switch" to optimize memory use within a 32-bit OS environment. If you get the 64-bit OS (avoid XP 64 if you can), don't use the /3GB switch.



Jeff Mowry
A people who value security over freedom will soon find they have neither.
 
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4000 parts?!?! This could be a good opportunity for you to develop your patience. As former President Clinton used to say: "I feel your pain." :)

The mech eng department that I work in uses 32 bit machines with 4GB and the 3GB switch, decent processors and graphics cards, good SW practices, but still struggle with assemblies and their drawings.

Lightweight mode can help but be careful with it. Pattern sub-assemblies as much as possible. Suppress fastener threads and other non-critical features. Saving assemblies as parts can help but when the assemblies are updated then the part will have to be re-created also.

Good luck.

 
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We do use sub-assemblies and lightweight!

Saving the assemblies as a part? we tried this in order to send the assembly model to our customer and it increased in size for 6meg for the assembly to 45meg as a part.

Is there a way to save an assembly as a single part? basically as a "blob".
 
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Yes, you can save a assy as a part. You can even chose to incorporate only the exterior faces.

Timelord
 
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Saving an assembly as a part was suggested a few years ago by our VAR.

SW 2009 now has something called "SpeedPak" that might work even better for you. Take a look at the "What's New Highlights" under "help" in SW for details.
 
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I suspect that you may have chosen the wrong options in making the part from an assembly. I have a made quite a lot and they are usually around half the original size, but like Timelord suggested, they only show the external faces.

Definately avoid too many top level mates and using materials that have any transparency, the latter will even make orientating a single part that has a lot of features impossibly slow, remove the material and it spins so fast you can hardly see it!

Trevor Clarke. (R & D) Scientific Instruments.Somerset. UK

SW2009x64 SP2.1 Pentium P4 3.6Ghz, 4Gb Ram ATI FireGL V7100 Driver: 8.323.0.0
SW2009x32 SP1.1 Pentium P4 3.6Ghz, 2Gb Ram NVIDIA Quadro FX 500 Driver: 6.14.11.7751
 
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Remember this is mostly new!

Does top level mates mean mates in the assembly?

When i saved the assembly as a part i selected Exterior Faces. this gave me the 45meg file. i then did it again with the Exterior Components selected and it is 28meg.

I am going to look into the speedpak today.

when i tried SW in 2003 I came away from it with a not so nice attitude. Now trying it again I am getting the same attitude.

thanks for everyones help
 
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Top Level Mates does refer to Mates at the assembly level. The rule of thumb is not to have more than 300 Mates. Do you have a lot of helix-based threads, or other heavy-processor type features in your part models? Perhaps a lot of in-context relations to other models? These types of things can slow down performance considerably. You could try to create simplified configurations of some parts to hide a certain amount of detail at the top assembly level.

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

Have you read faq731-376 to make the best use of these Forums?
 
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when i tried SW in 2003 I came away from it with a not so nice attitude. Now trying it again I am getting the same attitude.
Click to expand...
That's probably because you need some basic training. If your company can afford it, get training from a VAR, or purchase a subscription to SolidProfessor or myigetit. Both are relatively inexpensive and well worth the cost.

At the very least, find and join a SWUG for your area. The group will contain very helpful people.
 
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