SW suitable for large machines?

Would SW be the a good choise among mid range MCAD software for designing
machines that will contain maybe 40-50.000 parts when grouped in the full
mill layout? Made mainly from welded structural steel profiles and sheet
metal, filled with standard oem machine parts.
Have any of you got experience with this amount of parts, or have you run
into any limitations with less or more parts?
/per

 

I think one of the big Japanese companies did a presentation on this at
the 1999 SWW. They were building big steel mill equipment. They were in
the 20,000 part regime.

I ran into real problems with 5,000 parts in a large storage silo
system.

1. Extremely slow performance on drawings, especially sections and
multi sheet drawings
2. Difficulties with hidden line bleed through on large diameter thin
parts.
3. Problems with textures causing extreme performance degradation. I
had a texture on a shear stud that was used many times over.

Some of the solution to give a great deal of performance increase was:

1. Remove all hardware (nuts, bolts and washers) from the global
assembly.
2. Make sure all mates were good. No cherries.
3. No floaters.
4. Defeature any part detail that won't show up in the global drawings.

5. Work in shaded mode on drawings if you can. Also work in draft mode
as long as possible. In 2006 I don't think this is an option.

In my case this involved a lot of rework. The defeatured configurations
need to be made as early as possible in the modeling phase. It also
helps to have a consistent configuration naming convention for
defeatured configs and assmebly configs without hardware. Cherries need
to be avoided or fixed any time they show up.

At the 20,000 part and up level you may be looking at a 64 bit system
with lots of ram just to load the parts.

 

I've got no experience with large machine design, but how well SolidWorks
handles parts is strongly dependent on the type of parts. We have an
assembly with just a few hundred parts that brings SolidWorks to its knees
on machines with 1.5 or 2 GB of RAM. It works OK, but slowly, on a machine
with 2.5 GB of RAM and the 3 GB switch set. We've never tried doing a
drawing of it, but I suspect it would not be a happy experience.

I'm pretty sure that I remember someone in the news group saying not too
long ago that they were successful with 10,000 part assemblies. Other
members then chimed in to say how much trouble they had with less than 10K.

You really ought to give some serious thought to going with Pro/E, Catia, or
UGS. You should certainly set up some kind of benchmark test that gets
reasonably close to the type of work you want to do.

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

 

We hit the wall with IronCAD with 7100 parts. Even with 4GB and the 3GB
switch activated it can not generate any drawing views without "memory full"
errors.
Next we will be looking into Solid Edge, they seem to make a big number out
of their large assembly tricks, claiming to handle100.000+ parts.
But I wanted to check with you guys if you would say; no worries, that we do
all day, so I don't miss anything I should have seen. But no such response
yet.
Thanks so far.
/per

 

I was going to recommend Solid Edge, but looks like you already found it

Ken

 

I'm just curious how you will check out that claim. I think SW makes
the claim that they have improved the performance of SW on large
assemblies. Claims and reality can be two different things. And since
the SE usergroup is not an open group you really can't get the kind of
feed back you get here for SW.

 

I just checked the news groups for anything on SE that would answer
your question. There is very little if anything that I can find in the
"public" domain. I tried to stay away from comp.cad.solidworks
responses for the most part.

One other thing I will say, and I think it is in one of the threads
here also. SE has fewer VARS. That is my experience also. I wanted to
upgrade my seats of SE and couldn't get a response from SE in time to
meet my deadline. In the past I have asked them for quotes for other
types of FEA related software they sell. I got the quote the same day
the software I purchased arrived. I was too little a fish for them.

http://groups.google.com/group/comp...e+-cheap+-price&rnum=2&hl=en#34ae28fa47b19bcc
http://groups.google.com/group/comp...e+-cheap+-price&rnum=3&hl=en#da1eb0082de7fa42
http://groups.google.com/group/comp...e+-cheap+-price&rnum=4&hl=en#bad103654bd623e0
http://groups.google.com/group/alt....e+-cheap+-price&rnum=6&hl=en#e4ecd3c1330632df
http://groups.google.com/group/alt....e+-cheap+-price&rnum=8&hl=en#78bd4805a2971c9c
http://groups.google.com/group/comp...e+-cheap+-price&rnum=3&hl=en#1d963f72e8a2a293
http://groups.google.com/group/sci....e+-cheap+-price&rnum=4&hl=en#7fb4bf02503da8c8
http://groups.google.com/group/micr...e+-cheap+-price&rnum=8&hl=en#abc761e6ac5c1217
http://groups.google.com/group/comp...+-cheap+-price&rnum=13&hl=en#664f610bdd722212

 

I just called up a contact in a big SE site.

He regularly does 200-500 part assemblies. Here is his comment:

"It can be slow. It depends on how much detail is in the parts."

Once in a while they assemble all these small machines together to show
the assembly line. It gets slow. They are on SE16 and this user keeps
up with SE through user group and SE seminars.

I asked about the simplify function in SE and he said they don't really
use it alot, but it does help. For the SW heads, SE has a feature
called simplify that allows users to remove a lot of performance
robbing features for things like assemblies and drawings. It isn't much
different than a defeatured part configuration.

He summed up by saying that in SE it is somewhat user dependent as to
what performance can be obtained in an assembly.

 

All cad programs have some difficulty with large assemblies and while
some claim that they handle tens or hundreds of thousands of parts, the
reality is they all use some sort of tricks to prevent loading
something into memory.

UG uses partial loading, similar to Solidworks lightweight. For really
large assemblies, you can buy an advanced assembly license which gives
you some features:

Linked Exterior - Extracts Exterior faces.
Representations - Faceted wireframe model.
Simplified Assembly - Kind of like the Join feature in swx but stored
in the assy file.
Product Outline - Seems to copy the bodies into the assy file itself
but they are not selectable in any way. Purely there for visual
purposes.
Wrap assy - Creates a rough faceted wrapping around the assy. Doesn't
really resemble the parts, kind of like putting a bag over them, more
like rough volume.

All of these functions require setup and the use of Reference Sets
(Something similar to configs). There are no part defeaturing functions
as far as I can tell and there are no configs in UG. You have part
families but it saves each one of these to an external file.

So, as you can see, it's not loading all those parts.

 

I believe the ProE architecture also saves "configs" as separate files.
There is something to be said for not carrying the baggage of, say,
1,000 design table configurations into an assembly. Scott Baugh once
came up with a very definitive problem in that regard. The rest of the
things on your list can be done in SW with some work on the user's
part.

The defeaturing or simplify was in SolidEdge. In SW I just create a
derived configuration and start suppressing.

 

... I believe the ProE architecture also

If family table part or assy equates to "config"; no, it's all in a single file.
Possible you mean Simp Rep? They can be internal or external.

Pro/E (entry level package) offers a few ways to help deal with large data sets.
They all require setup and some degree of user expertise (any schemes that claim
not to, I'd look at with a jaundiced eye) but the basic Simplified Rep is
effective, versatile, simple as picking parts not to load or to load graphics
only or geometry only component reps. Query building functions and rule defined
reps can help, too. Components can be loaded or unloaded from memory as you
work without creating xref dependancy problems. Envelope parts and Shrinkwraps
require a little more work and user knowledge to set up but allow for more
versatility and a greater potential for resource savings. If large assy
performance for mid range price is a criteria it's worth a look.

 

Anything with that many configs is probably a very simple part anyway,
mostly stuff like fasteners and other standard parts. I did some
testing a while back and saw no slows down using configs versus
individual part files. We commonly use our library of fasteners, some
which contain 250+ size configurations.

It wouldn't take too much effort on Solidworks part to add similar
functions. When you do a "save as" on an assy and change it to a part,
you have similar options already, now if they would just link it so it
stays up to date, or store the 3d body in the assembly file as a
feature that can be referenced by other top level assemblies.

 

I thought Pro/E did family parts as separate files too. Did they change
it recently?

 

I thought Pro/E did family parts as separate files too.

Well, actually; it can -- sorta. By default it doesn't. (Default settings also
show table instances in dialogs; i.e. file open or component placement, which
can lead to the impression that instance part files exist on disk) It can be
configured to save .xpr "instance accelerator" files. They are intended to
speed up retrieval (says the documentation) so I guess you can say it does ...
in a way. The parent generic / table file must be accessible to load an
assembly containing instances (.xpr's don't appear to be "stand alone"). I
don't know if they have a significant affect on consumed resources when an
assembly is loaded. It may have been done differently in the past; my
experience only goes back a couple of years.

 

Scott's benchmark problem actually had what amounted to a single part
or very few, but the part configurations were all used to populate the
assembly. One part, many configs all used simultaneously. My
experience is that this kind of construction technique still will weigh
down SW.

 

I want to summarize a few things.

1. The consensus is that SE is certainly not an order of magnitude
faster than anything else out there as the 100,000 part assembly claim
might lead one to believe.

2. Working with models as large as you intend to do will require as
much from expertise as from the software.

3. Some software has no chance dealing with what you intend to do.

4. SE is a little clunky in the way it does mating (or placing as they
call it.)

1. If you are going to get into assemblies this big it will be just as
important to have someone on your side who knows how to get this done
as it will be to chose the software. Whether this is a VAR or a
consultant like Matt is up to you.

2. The choice may come down to secondary issues like modeling speed,
ability to import parts, VAR support, etc.

 

Sorry, this turned out to be an extra long post, most of which is
available in user group presentations on my website
http://mysite.verizon.net/mjlombard/ in the User Group area.

Success with large assemblies in SolidWorks is mainly dependent upon a
combination of technique and settings.

I was just working on a 2 part assembly that because of a bad technique
I used "just to get the job done", gave me some bad rebuild times, even
on pretty good hardware. I was able to make some settings to offset the
effect of the bad technique.

Most of the problems I see with people having trouble with assemblies is
avoidable and self inflicted, even though most people blame the
software. I guess that's the easiest thing to do since you don't
generally have to learn anything to blame the software. Because of
that, take criticisms with a grain of salt, especially impassioned
criticism.

There are a lot of things you can do to paint yourself into a corner in
SW, and not all of them obvious. Is it the software's fault if it
offers good and bad ways of doing things, and doesn't help you
distinguish between them? Sources of truly reliable and comprehensive
information are few and far between, particularly around assembly
performance. If you know what you're doing, you don't have to pay the
price of bad modeling techniques, but how do you get to the point where
you know what you're doing? SolidWorks training doesn't even begin to
cover it. Also, you have to come to grips with the fact that you are
stuck with the limitations of the software you are using whatever it is,
and learning how to work with/in spite of it

From what I see, Pro/E has a clear advantage over SW in large assembly
capability, but there are other things about Pro/E which make it less
attractive. The ability in SW2006 to turn off automatic rebuilds will
be a big step forward once I start using it.

The original post was about structural steel (I read "weldments" here)
and sheet metal. I personally love the sheet metal functions in SW, but
I'm just a plastics guy, so I don't really know any better. Weldments
in SW can be handled primarily as multibody parts, which may be an
advantage and may not. Big perforated patterns in sheet metal are one
thing that will bring SW to its knees quickly. The technique here is to
have a simplified configuration.

The sooner you realize that you're not going to work on detail parts in
the 50,000 part top level, the better off you'll be. In large
assemblies you will work with several ideas:

- break large assemblies into subassemblies where possible to limit the
number of mates and assembly features solved at the top level

- use patterns effectively. instead of mating 10 screws, 2 mates each,
mate just the first one and pattern the rest. using hole wizard for
holes can help you make feature driven component patterns, even for
irregular patterns.

- limit the use of incontext features, and lock them if you can. You
can't unbreak a broken reference, but you can unlock a locked reference.
same performance benefit.

- absolutely avoid circular references

- don't mate to: assembly features, incontext parts, assembly level
reference geometry created with some reference to a part, pattern
instances

- fix errors as they happen

- avoid flexible subassemblies if possible

- make use of simplified configurations in parts and assemblies.
There's this great technique which I've never heard of anyone using. If
your parts all have a config with a certain name like "simplified", in
the open dialog you can create a new assy config that automatically
references all the part configs with that name.

- SW2006 has display states which are much faster than configs for
controlling visibility

- Don't scoff at lightweight. If you are using large assemblies in SW,
you need to be using lightweight. This gets better literally with each
new release of SW.

- Don't be afraid of Large Assembly Mode. just understand it for what
it is, a different set of performance settings that kicks in either
automatically or manually.

- Display settings are important. Use common sense.

- Avoid transparency, wireframe, section views, curvature, zebra
stripes, etc. That isn't to say "don't use" these things, just realize
that they are going to cost you something which may or may not be worth
the benefit

- Turn off "update mass property data"

- Turn off anti-virus real-time scanning. You may have to strangle a
rabid IT person to do this. Sacrifices must be made...

- Work locally. Get a PDM system to share data. It's not impossible.
Figure it out. If you can't, hire someone who knows what they're doing.

- Get a fast hard drive

- Don't skimp on ram

- Don't open files by double clicking in Windows Explorer - use the Open
dialog

- Turn off the back up and auto-recover functions

- Realize that using Toolbox over the network is probably a performance
mistake

Large assemblies are managable in SolidWorks, but you have to accept
that you will have to actually plan your approach. Good things won't
happen by accident. There is no "easy button". Some useful techniques
that you see all the time in sales demos and training classes are
actually bad ideas. Be very careful about who you take ideas from.

 

Sorry, this turned out to be an extra long post ...

Au contraire.
Good article and advice.
Applicable, more or less, to any system.

 

In Scott's case, most of the single file, multi config parts were mated
to each other. It could also be that they fixed this in 2006. I'll
have to check.

 

Matt,

This is some very good information. I don't deal with assemblies near to
the scale of what this thread is discussing. But this info will still go in
the "keep" folder.

I do have one question though.

">- Don't open files by double clicking in Windows Explorer - use the Open
dialog"

I am curious. What is the reasoning behind this? I almost always use
Windows Explorer to open all of my files. I have never noticed any
differences in speed.

The only problem I have ever run into using this method is when I open
multiple files simultaneously. If for example I wanted to open 10 SW
files, I used to highlight all 10 of them, right click, and select open. At
some point (I think when SW2004 came out), when I tried this method it would
not work. It would only open the first file. After that, no other file
would open regardless of what method you used, until you closed SW. Then,
by itself, SW would automatically re-open and load the second file, only.
Until you closed it again and it would re-open loading the third file, and
so on.

The workaround that I found was to highlight all of the files from Windows
Explorer, and drag them to the SW window. I would drag them specifically to
the SW window title bar. I have never had any problems with this method.