Large Assembly / Performance tips needed for user group presentation

I'm at it again. Last time a bunch of people helped me out with an
advanced design table user group meeting, and this time I need some tips
for a large assembly user group meeting.

Last time I think a lot of people (including me) learned a lot just from
the exchange of ideas, and I hope this time can be the same.

I'm looking for practical things that you do to work with large
assemblies. Anything from hardware to OS set up, network, to SW
settings or whatever.

Thanks in advance!!



I'll start with a quick list

- simplified configs of parts and assemblies
- turn down assembly image quality and tell it to use the same setting
for all parts
- use lightweight parts when possible
- use LAM when possible, and understand how it works so you can over
ride its settings when you need to


matt























matt

 

The biggest, baddest, bestest thing I can think of is to turn on the 3gb
switch. I have been running it for a few weeks now, and just about every
day, I could not have done the stuff I did without it. The imported car
bodies I have been working with have pushed me all the way up to 2.6gb
Commit Charge. Obviously, this would not have worked without the switch
turned on.

I know, not exactly what you were looking for, but it was what let me do my
job for the last couple weeks.

WT

 

Here is my dozen.

1. 3GB switch as has been mentioned.
2. At least 2GB ram. SW seems to use large amounts of ram temporarily even
though when quiescent it may indicate well below 1GB. With 2GB physical ram
and the 3GB switch SW will max at about 2.6gb before terminating.
3. AMD64 FX53, FX51, 184 seem to be the fastest hardware.
4. NVidia FX series video cards also help.
5. Run the video resolution down as much as is tolerable:
a. 1024x768
b. set document properties to fastest while working.
c. turn off anti-aliasing
d. work in shaded mode.
6. The new SATA hard drives are very fast.
7. There is an article on the SW forum about how to put together a very fast
network setup which includes dual gigabit ethernet and other goodies.
8. SAMBA on Linux seems to be a very fast server.
9. Keep the assembly clean. Bad mates should be fixed when they occur. They
seem to cause instability and slowness.
10. Avoid large numbers of patterned flexible assemblies. Having many
duplicate configurations of the same sub assembly will greatly slow
assembly performance.
11. Avoid large numbers of the same part with different configurations.
12. I find the Spaceball to be invaluable when mating due to the ability to
pick up a part and move it into position while rotating the view with the
mouse.

 

Wake up, boy - Large Assy Mode....

WT

 

I know that hidden parts still carry some baggage, but with the car body
files (20-80meg) I have been dealing with, I could achieve 10 fold
improvement by only hiding them. My thought is this. As I rotate and
manipulate the assy, all the imported surfaced body info doesn't have to be
handled with the video. If I suppress them, then I have to wait for them to
load again when I do need them.

I also noticed that shaded with edges was dragging me down with noticeable
delays, but when I switched to plain shaded, the delays were gone. I still
like the edges on, for the most part, but will turn it off when I have the
bodies showing.

WT

 

Hi

What is the 3gb switch?

Anders

 

Sorry, I just couldn't pass that one up - too easy. )

WT

 

Matt,
Here's a couple for the "what ever" category.

Get used to it. Depending on your set-up, large assemblies can (and will) be
slow. Look for other things to do during long rebuilds, loads, or mates.

Turn off things like view animation, mate animation (uncheck "preview
mates"), don't use transparency.

Get a PDM system and run files from your local drive.

Richard

 

I like that. It goes well with your crashing presentation called "It's
your fault". You trying to get me hurt?

Thanks for the suggestions, people have to admit at some point that reality
exists.

matt

 

Thanks for the list! OS, hardware and network settings are certainly
valid.

How is that group going? I've heard good things about it from some jealous
RUGS (Rochester user group for solidworks) members.

You didn't call it "BUGS" (Buffalo user group...), by any chance, did you?

Thanks again!

matt

 

Whenever people ask me about this, I point them to your website. I guess
that isn't too much help in this case!

We don't deal in really large assemblies, but our complex part shapes cause
a lot of the same problems in smaller assemblies. I've got to think that
going back to SW03 might not be such a dumb idea. The bloated file size in
SW04 is driving us nuts. Does it cause problems for large assemblies as
well?

Jerry Steiger
Tripod Data Systems
"take the garbage out, dear"

 

"Jerry Steiger"

Actually, it did help. I had forgotten I had that up there. Thanks for
the reminder.

Thanks to all who posted something. I think I used some of everyone's
suggestions. The presentation is up on my website now, if anyone is
interested.

www.frontiernet.net\~mlombard

Go to the Rules of Thumb link, top of the list. RMB on the link to save
the file locally, other wise it will run powerpoint inside the IE frame.


matt

 

thanks matt,
I have found screaming at the software to be very therapeutic... : )

 

Matt,

When your "research" can you publish here your findings?

Thanks in advance.....

 

Hi

I always turn off cosmetic threads in assemblies.

Kind regards
Klaus

 

www.frontiernet.net\~mlombard

Go to the Rules of Thumb link, top of the list. RMB on the link to save
the file locally, other wise it will run powerpoint inside the IE frame.


matt

 

Thanks for that, Matt

Nice job. It's excellent to be given access to such a comprehensive and
compact resource.

 

Matt:

Here's one that I found recently that may help in some situations
where you just can't seem to open an extremely large assy, even with
4GB RAM and 3GB switch.....(or with less RAM of course)

Usually this is a technique that comes in handy for fully resolving an
enormous assy for the purpose of checking in to a PDM tool.

Some assemblies can't be opened fully resolved without running your
box out of memory. What's interesting is that I've seen SolidWorks
memory usage soar while opening, only to drastically drop after it's
finished -- leaving you some memory to continue. So you open them
lightweight - I find that setting LAM to auto-lightweight is the way
to go. Then, you open the assemblies one-by-one in their own window
and then fully resolve them. The mem usage will spike and drop, spike
and drop, etc as you do this. It's kind of like using a rachet jack
to jack up your car. Doing this I've been able to fully resolve
assemblies that were otherwise impossible to check in.

It's still painful, but it does work.

Todd

 

For checking in large assemblies with the PDM (DBWorks) I've also
found that it helps to open the assembly file, fully resolve all the
components, then open the drawing file, lastly Check-IN the drawing
file...and the assembly file automatically checks in after the drawing
file.

Ken