SW2003 Performance 5

[BBJT]

Does anybody have any input on the performance of 2003 yet. I have seen out in a couple of other forums that the sketcher is really slow.

I have not run into any major issues yet but I am a far cry from a power user.

Any feedback would be appreciated. The users here have started beating on my door asking when they can have it.

BBJT CSWP

 

[Standing]

BBJT,
We have 19 SolidWorks users. When SolidWorks released SolidWorks 2003 SP 0 I jumped on it. A lot of things changed for the better. I have not noticed any change in speed, slow or fast. I never did time SolidWorks loading before or after the upgrade. I thought SP 0 was the released version. It is too late to go back to SolidWorks 2001 Plus SP 5.1 now. Now I am hoping nothing immense happens. I am having trouble opening some large assemblies, which could easily be opened with SolidWorks 2001 Plus SP 5.1.
Bradley

 

[BBJT]

Thanks for the feedback. I have been pulling up assembles with three thousand parts and have not crashed it yet. I was pulling them up to make sure that we did not have any mating problems like we had going from 2000 to 2001Plus. I am going to try and pull up a smaller, maybe half that size, and edit a part and try sketching to see if I see the slow down that is being reported in other forums. BBJT CSWP

 

[Standing]

BBJT,
I have heard that companies can open large assemblies. We never have been able to open an assembly with 2000 parts. We put in a 1-gig network line, with a 1-gig network card. The fastest computers at the time of 1.7 gigs, with 2-gigs memory, G force approved video card. I put the assembly on my C:\ drive I still cannot open the large assembly. We do use external references and configurations. I have talked to tech support and set all the options they suggested without any improvement. How do you do it?
Bradley

 

[BBJT]

We are on what ever PC IT throws at us when it comes time for upgrades. They are useally the latest and greatest compact. Because I was upgrade last year I am only on a Pent 1 GIG with 512M ram. Granted if I do not load the assembly light weight I start swapping due to the lack of memory. Our network connection speed 100 Mbps. I did a recent test between opening a 3000 component assembly locally (hard drive) verses loading it form the network, to my suprise the difference was minimal.

What do you mean by you never have been able to open 2000 component assemblies? Are you crashing SolidWorks? Is it hanging? Does it Lock up the system? BBJT CSWP

 

[Standing]

BBJT,
My SolidWorks hangs up while opening large assemblies using none lightweight. When I look at the task manager, SolidWorks is not responding. I know that this is not a good test. If I look at the task manager on medium sized assemblies, task manager is also saying not responding. Then all of a sudden SolidWorks will complete the open. I let SolidWorks try to open on a day I took off work. Started opening at 4 pm on Tuesday and on Thursday morning the file still was not responding. I tried opening lightweight and the assembly model opened. Now I have not made a drawing of the assembly, but I think when opening a drawing the parts have to be resolved. I am giving it a try now.
Bradley

 

[Timoteo]

Experiences with our clients reports:

- SW 2003 is 30% slower than SW 2001+.
- The hardware is the same, the operational system is the same. Why SW 2003 get slower???

I hope someone could explain to me...

Timoteo

 

[josephv]

Hello Bradley,

We can open assemblies with over 200,000 components. To do this we use best practices:

1) Use simplified configurations (suppress extruded text, cosmetic fillets, threads, detailed features), this reduces the quantity of OpenGL triangles that the PC has to process
2) We use Windows 2000 SP2 or XP (note that NT and Windows 2000 SP1 had limitations with file size)
3) Lock External References
4) Use Large Assembly Mode and Lightweight
5) Always open from the local drive (luckily PDM/Works does this automatically)
6) We suppress internal components (using advance select), suppress removes components from memory.. hiding does not..
7) We resolve all rebuild errors, including imported files
8) We only use video cards designed for CAD applications like the nVidia Quadro, Oxygen 3DLabs, or ATI Fire GL8800.

Hope this helps... if you continue to have problems you may want to bring in you reseller to help troubleshoot your assemblies.

Joseph

 

[josephv]

Hello Bradley,

I forget to mention three other important best practices:

1) Use Fast Image Quality, this also reduces the OpenGL triangles (i.e. quantity of data to be processed by the system)
2) Always turn off the virus checker and other programs when installing SolidWorks or any Service Pack, otherwise the virus checker will block the install of criticall DLL files resulting in performance and stability problems.
3) Always get the latest video driver before installing a new version of SolidWorks.

Hello Timoteo,

Your clients mentioned that SolidWorks 2003 is 30% slower than SolidWorks 2001Plus.

Please ask them "Which operations are 30% slower? Is the problem file specific?".

We have tested several operations and assemblies (e.g. file save, open, rebuild, rotate) and actually found SolidWorks 2003 to be faster.

As I mentioned to Bradley, make sure your customers disable the virus checker when installing SolidWorks, and ensure that they are using the latest video drivers (hopefully they are using video cards designed for CAD applications)

cheers,

Joseph

 

[BBJT]

Josephv,

2) Always turn off the virus checker and other programs when installing SolidWorks or any Service Pack, otherwise the virus checker will block the install of criticall DLL files resulting in performance and stability problems.

Turning off virus checkers is OK for companies that have the ability to do this. Working for a large corporation such as mine we are locked out from turning the virus protection off. Do you get errors if one of these critical DLL's don't not load correctly? How do I know SolidWorks is installed correctly?

We can open assemblies with over 200,000 components
WOW! What kind of load time are you seeing? I am guessing hours. A total machine layout for us could run from 30,000 to 100,000…..components . The computer hardware seems to get better everyday but I do not believe that it is good enough to build these large assemblies in a timely matter….yet.

We suppress internal components (using advance select), suppress removes components from memory.. hiding does not.. I like this idea. Could you elaborate on the advance select a little more? How do you select internal components only?
So when you open your 200,000 component assemblies are you really opening all 200,000 components or do you have a large amount suppressed? Again I am very interested in how long the load time is on an assembly of this size.

Have you thought of publishing a Best Practices book for large assemblies of this size? It sounds like you have a lot of tricks up you sleeve that would benefit all of us. We do most of the things you mentioned above today. I am thinking that the advanced selecting the internal components may be the part of the puzzle that we are missing.




BBJT CSWP

 

[Standing]

Thank you Joseph,
Ideas like yours are exactly what I have been looking for. We have never turned off virus protection. I will do this from now on, along with the other suggestions. I thought I studied SolidWorks. How do you find these ideas, like “Lock External References”? I would never have thought.
Bradley

 

[josephv]

Hello Bradley,

Luckily, my company has sent me to training and seminars. This is were I picked up most of these tips. SolidWorks World has many seminars on large assemblies.

Hello BBJT,

If SolidWorks was installed with the virus checker turned on, there are so many things that can go wrong. I wouldn't even know were to begin. A couple things that can go wrong is constant crashing, poor performance, not able to save an eDrawing, math operations don't work.

My advice, please ask your IT department to turn off the virus checker during software and Service Pack installs.

I would never open a 200,000 component assembly fully resolved (there is not need to). I always open an assembly configuration called skeleton that has a layout sketch of the assembly, where most subassemblies are suppressed (including internal components), and I only unsuppress the components that I need to work with.

To suppress internal components... Tools > Advance Select > under Property select Part is interior detail -- SW Special...

I will be writing some magazine articles on Large Assemblies, once I have finished them I will gladly send everyone the link.

cheers,

Joseph

 

[BBJT]

Joesphv,
Thanks for the tip on the Advanced Select. I was not aware of the select Part is interior detail -- SW Special option. I was afraid that you were going to say their needs to be a property set up in each file in its own config. I am going to play around with this a little and I will let you know if this will work within our company.

Thanks again for the excellent feedback.
BBJT CSWP

 

[Standing]

Joesphv,
Can you open an assembly drawing with over 200,000 components, using SolidWorks 2003 SP 0.0?
Bradley

 

[roboeng]

Is the Part is interior detail - SW special option on in solidworks 2003.

 

[josephv]

Hello Bradley,

The assemblies with 200,000+ components were done a while back. We started the project with SolidWorks 2000 and completed in with SolidWorks 2001Plus.

We have not worked with them since, but we have tested 50,000+ assemblies with SolidWorks 2003 PreRelease and SP0.0, with very good results.

Here is another good tip that helped us...

1) For subassemblies with several components and many assembly features, JOIN it into 1 single part and LOCK the external refernces (this is similar to the new shrinkwrap functionality, but I like JOIN better because it is parametric i.e. if the assembly changes the JOINED part updates).


Hello roboeng,

Part is interior detail was introduced in 2001Plus.

cheers,

Joseph

 

[Standing]

Joseph,
Thank you so very much. Bradley

 

[roboeng]

Thank you Joseph Your tips are very useful.

 

[Mindnumb]

Sw2003 Seem to not use hardware open gl !

I compared it to sw2001plus, and its so slow !

When I check the software acceleration checkbox on both 2001 and 2003, its the same perfomance, but when I uncheck them, 2001 get enormous performance boost, and 2003 gets even slower than on software.

Its wery frustrating !

Im am currently using a asus GeForce2 GTs With Quadro hacked drivers ( 30.82 ) .

Next test is to uninstall the quadro drivers, and install
the good old vanilla nvidia drivers, but then I will get a serious performance hit because of the unified back/depth buffer thing.....

Help....

 

[BBJT]

Well,
So much for the Advanced Select, Part is interior detail -- SW Special option. Configs, configs, configs. Because SolidWorks does not save assembly specific info in the assembly it applies to you are forced to create configs in every part and assembly that you create. The problem is when you suppress a part in a sub-assembly it has to write back to the sub which in turn suppresses it in all the other configs of the main assembly and where ever else the sub is being used. AHHHHHHHGGGGGGGGGGG!
BBJT CSWP