Large Assys - SW Not Proven at All

I would have thought this information would be easy to find, but it has
been quite the ordeal. It relates to the handling of large assys in SW.
We have a large assembly line with roughly 100 000 parts, about 60 000
non-fasteners and roughly 30 000 unique components. We are seriously
considering SW, but have seen no proof that SW can handle assemblies of
this size. I understand proper assy practices need to be used and very
powerful computers are required, but I have never heard of anything
close to even 30 000 components.

SW has shown close to 10 000 part assemblies in demos and claim they
can do more, but I hear a lot of talk in forums about headaches people
are having with large assys (even 5000 parts!!!). So what I'm asking
is this:

1) Can you refer me to any companies that are designing very large
assys with SW?
2) Is the SW engine inherently limited in handling large assys by
design (i.e. will the program grind to a halt at a certain point,
regardless of hardware)?
3) Isn't managing the simplified versions of parts and sub-assys
difficult and doesn't it introduce additional potential for errors?

We are considering Catia as well, but are worried it is overkill for
the machine design we're doing. I'm very interested in hearing your
experiences.

Thanks,

Mark.

 

If you want to talk to a user who is designing things with 100,000+
parts, go talk to Boeing, Airbus, or maybe the largest factory
automation companies. An airliner can have about 1 million components
from what I remember from press articles.

I think the CAD packages used at the top of the heap will be very few.
They will also be linked via mainframe in a large LAN/WAN.

That being said, I had an automation system quoted from a large
automation company (500 engineers) that was NOT using CATIA or similar
highest end CAD systems.

Why?

The answer was that everything in my case was modular. The typical
modular system is components placed along a "track", and there is no
need for them to build the whole system in one "assembly file". They
used a 2D layout and bought or made the modular components.

There are several ways to skin the cat, depending on whether you are
looking for eliminating a pest or getting dinner.

 

Mark,

That's a hell of alot a parts. Your going to have to be very organized and
modular in your approach regardless of the system you use.

I don't know that I'd want to attempt to do such a thing in SW. Catia has
tools to handle this kind of data, so does UG. Even with these systems
you'll be using tricks to manage it. It's not overkill if it will work, and
others won't.

Software quality seems to be pretty poor these days, over all. No matter
what you decide you'll probably have problems.

Regards

Mark

 

Mark,

I don't believe you will find companies working in the 100,000 part range
with Solidworks. Right out of the gate, you're probably better off with
Catia and likely a non-MS OS.

There are some techniques that you can use to make assemblies in the 10,000
part range usable in SW, and likewise, it is possible to construct
assemblies with 3 or 4 parts which are terribly slow. It's all based on
either good or bad technique. I'm not sure that an assembly of 100,000
parts will substantially benefit from technique.

Simplified configs are certainly one of the techniques you could use,
particularly with subassemblies which helps large assemblies become
managable. It's usable, but not foolproof.

 

Based on my experiences with large assemblies you'll likely have major
problems if you tried creating a 100,000 part assembly with SolidWorks.
I wouldn't say it's impossible but you'd need some sort of super
computer to get anything done. That's WAY out of SolidWorks's league.

 

Performance is the hot topic across the mid-range board these days.

I don't have any first hand experience, but think you are talking outside
of, or at least on the fringes of, mid-range CAD / Windows / PC
capabilities for all (or most?) practical purposes.

To get a little perspective search the web for Epaq Care Solutions and
Itanium. Epaq had a half million part assembly that was the subject of a
lot of PTC marketing literature about a year ago. I was wondering about it
a few days ago and did some searching and couldn't find anything more
recent on it. Broke the company, done with and good riddance...? I have
read that PTC has more or less divorced itself from the Itanium, but don't
know where it's gone instead.

Just curious, how are you currently handling the designs? Still on 2D
acad?

Good luck with the quest.

PS Just to add a bit of hearsay to muddy the waters; I've read that Catia
5 is no fireball. Might look into that.

=========================

 

I am using Solidworks, an assembly with 800 parts, excluding fasteners, runs
like an old dog, I was using about 20 mirrored parts , but changed them to
normal parts,(by remaking them).

The assembly now runs a bit faster, but, and a big but here, is that if any
part has patterned holes, these have to be suppressed, for the assembly even
to open in under 25 mins.
This means adding a note to the drawing document, to tell the shop floor,
that this drawing is incorrect and should include patterned holes!
Which means, enabling the patterned holes in the part and reprinting. Even
worse is somebody else printing out the drawing documents!

If I wish to change a part design, (that is in the assembly), 30 seconds to
1 min wait times for the change to complete, are normal.

I am NOT using in-context parts, multiple configurations or mirrored parts
in this assembly, all sketches are fully constrained and all parts are fully
constrained in the assembly. But the interesting thing, (in the drawing
document), is that in adding, the very first dimension and every dimension
after I get the over-constrained dialogue box, huh?

The only thing that I can see for this slowness, is that the parts were
made, using 2005 sp0.0, templates. which have known problems.

When I get the time, I will redraw the parts, using 2005 sp 2.0, templates
and see what the differences are.

Why?
Because I hope that Solidworks will improve, It is a very easy program to
use, even though the help files are pants, (try looking for design library),
then look for library, huh?), lol @%7^$
The support is great, with the added bonus, of some very clever peeps here
to help.

I would love for someone to send me a file with 10,000 parts in it, plus
drawing files, to see if this really can be achieved or even has both the
assembly document and the assembly drawing document open at the same time!

BTW, my pc, is above average spec, can get better, but would need about
£6000, to get to Nvidia fx4000, 4Gb ram, etc....
My PC is way above, what Solidworks recommends, for 800 part assemblies.

Whoever you choose, get them to show you an assembly, having the number of
parts, in it, that you will require.
Even more important, is that they show it to you, on your machine, not
theirs.
With your machine, setup in the way that you will use it, after they have
gone, otherwise, you will be on to support, every day.

Going to use Pdmworks or another pdm system?, include this in the setup
Exporting or importing to DWF, CAM?, get them to show you, test the output.
PDF files, importing into word, Edrawings or similar, FEA, printing out to
more than one printer, etc.....
All these need to be looked at and shown, do NOT take their word for it!
Can someone else, on another pc, open the file to check a measurement for
example, will this cost extra?

If they shy away from these requests, you can bet, it is because they know
it will not work, be very slow or require a lot of extra work.

Many talk the talk, but very few can walk the walk, lol

The best thing is to sit down with everyone involved and take notes of what
is required, you will be amazed at what you didn't think of!

Sales Pictures,
Service Parts drawings and part numbers linked to a machine made in 1917,
lol 8-\
Work shop drawings, pictures and manuals, i.e.: assembly procedures exploded
assembly drawings
Engineering, sheet-metal work, castings, out sourcing
Parts lists (boms)
Storeroom data
Drawing numbering, revisions.

Now that's the end of the gloom, I hope you had a happy Easter

 

No cad system can load up that many parts. They all use specific
functions to "try" and work on larger assemblies. These fnuctions
revolve around creating "representations", Linked Faces, "Lightwieght"
or something to that effect. Some softwares do this better than others.

I use UG and Solidworks. UG does have some "Advanced Assembly" options
that cost extra $$$$. You do have to setup these options ahead of time
though.

Product Outline: Just a boundary of several components, but the parts
aren't loaded, gives you an idea what's there.
Representations: Faceted bodies that are linked but not loaded.
Wrap assembly: Creates a solid at the boundary of several components so
it doesn't load parts.
Linked Exterior: Exterior faces of parts linked to the originals.

All these are just techniques in UG that keep you from loading so many
model files.

Solidworks doesn't have all these options but you can do some things
similar with configurations. Create simplified configurations in parts
with features turned off like fillets, chamfers, drafts and any other
internal detail features you don't need to show in an assembly.

In sub-assemblies, create simplified configurations with parts and
other sub assys suppressed, not hidden. Turn off fasterners and all
internal details if you can. Use Lightweight, it does help.

So when it comes down to it, no cad system opens that many parts, they
all use tricks to reduce the number of models being loaded while still
showing enough info to represent it. Your details will come in on the
sub-assys drawings, and their sub-assys, and at the part level. The top
level is simplified. What you will probably find is that no matter what
cad system you go with, you'll have to jump through these hoops, just
test them all to see which ones have the tools to get you there.

JC

 

Mark,

There are numerous customers using SolidWorks for large assembly modeling.
One of my customers successfully uses SolidWorks to model train locomotives
and railcars that contain over 60,000 parts.

Have your SolidWorks VAR get you some references. Several that come to mind
are Vermeer, Bucyrus, Haumiller, Automation Tooling Systems, Michelin, etc.
You should be able to find some reference information on the SW website.

You will hear negative comments on this, and other newsgroups. Newsgroups
are frequently filled with "this stuff sucks" posts. Rarely do users go to a
newsgroup to say how great their software is. Just human nature I guess.

BTW, what kind of machines do you manufacture?

I'd better put on my flame retardant suit now.

CAD Guy

 

Mark,

-----------------------------

The flame suit shouldn't be necessary, but some additional info would be
welcome....

Parts / part instances?

What type parts? Simple solids, feature intensive, sheet metal?

Unrelated parts or associative top down designs?

Are they happy with it all?

It would be nice if more of this info got out to the public.

==================================================

 

I personnally doubt if you if you could actually work with an entire 60,000
parts assembly at once. I would think that if you tried to open an assembly
of a domestic car (for example) fully resolved, you would run out of RAM and
the assembly would crash. I work daily with assemblies of about a thousand
parts, and I use about 2 GB of RAM. Once I enter into the virtual memery ,
the computer soon crashes. Today's PC computers are limited to about 3GB of
RAM. There's no way I can see you opening 60,000 parts on a PC Desktop using
SW.

 

I've met with some of the Haumiller people. They have their stuff
together. Unfortunately few "normal" SW users/companies are as
organized as they are or have the expertise they have. Which leads me
to believe that success with the software is at least as much a
function of company organization and expertise as it is with the
software. I don't think that the average VAR AE or TTM is on the level
of people like Haumiller in terms of making practical use of the
software. And if they aren't, it is pretty clear that it won't trickle
down to the user level.

At SWW I listened to the StructureWorks people talk about how they
handled 100,000 part assemblies and the hoops they had to jump through.


One thing is clear, that you have to trade off one feature for another
to get SW to handle these monster assemblies and that success with
assemblies is very much a function of discipline and planning early on.
I think it is also true that certain types of assemblies can cause
problems no matter what you do. Assemblies that use parts within parts,
aka, configurations are one example. Assemblies that tie parts together
with in-context features are another. Use of things like SmartFasteners
which can populate an assembly with thousands of fasteners very quickly
is yet another.

website.

 

It would be nice if more of this info got out to the public.

Absolutely. It's sad that most of what we have to go on is really costly
personal experience, vendor promotional literature (I've noticed that SE
has upped the bar to "massive assemblies" in their latest lit) and a
worthless industry "press". I wonder if any of the "cost you a couple of
hundred dollars" periodical publications have anything worthwhile in them.

Anybody got any links to more of these?
http://www.cadventureinc.com/white-papers/assy_perf_cubes.pdf
http://www.adi.bz/download/23982en_file1.pdf
I like to print 'em, put 'em in the john and read 'em at "leisure". In
retrospect it can be seen that a few "truths" can be gleaned from them.
Remember the "built from the ground up for large assembly performance" that
was so widely circulated a few years ago?

 

Kman,

No, this customer doesn't typically open the entire 60,000 part top level
assembly. They work smarter, not harder.

The engineering manager for this group came from a Pro/E / UG background.
He educated his SW users in the proper techniques to handle large assemblies
(skeleton parts, configurations, simplified representations, etc.).

They use top down modeling techniques where required, then break the
external relations when the design has stabilized.

Regarding you comment about sales people, while I agree that some fall into
that category, I have been doing this for 18 years, and am a certified
instructor and support technician. I was recently recertified for SW2005.

Some of us have a conscience, pride, and respect for our customers.

CG

These techniques should be employed regardless of what software is being
used.

 

The problem with the part Template, was with cosmetic threads, not knowing
if they wanted to show or not, lol
The feature (texture), was disappearing, when the part was rebuilt or
shaved.

The problem with the Drawing templates, was that adding dimensions, was
pulling up the over constrained feature manager!
and telling me that the part was over constrained.
When opening the part window, the part had changed and needed updating, lol

The problem with the assembly Template, is the time it takes to open, even a
5 part assembly!

I have since re-made the templates in 2005 sp 2.0 and everything seems to be
much better, but I will wait until I have rebuilt the whole assembly on this
service pack, before confirming everything is ok again.

 

Check out Solid Edge from UGS. The newest release (V17) has some new
features specifically geared towards massively large assemblies.

Ken

 

Any empirical data to support those big adjectives? You need to coax them
into publishing something. If nothing else they can at least add to
inventor's trouncing unless all that Functional Design stuff helps 'em
(darned sure don't want to overengineer all those cubes). 8~)

 

I haven't seen any numbers, but does that really mean anything? They can
tell you anything, but untill you try it yourself...

Ken

 

I haven't seen any numbers, but does that really mean anything?

"They" as in the numbers, or as in the sales reps?

There has to be some potential for ROI apparent before I'll spend the time.
Haven't seen anything yet to indicate there is any. Sooner or later
something will pop up. I'm sure there's a lot of this "testing" going on
behind all the various curtains. Of course no one's gonna publish anything
that indicates the other guy wins and there has to be justification for
buying the ad space...

 

In my experience SolidWorks is a huge resource hog.

My performance reference is Pro/E.

SolidWorks slows to a crawl displaying hidden line or wireframe views,
even on relatively simple parts. Drawings are slow to manipulate.
Assemblies over about 500 parts slow down to a crawl. File sizes are huge.

There are tricks to help but these are basic problems.

I use SW every day and I like it, but it is not the kind of program you
would do anything too serious with (no cars, space shuttles, planes, or
nuclear submarines, etc.).

Part of this is due to the Windows-PC platform to which SW is married.

I'd suggest looking into a very fast 64-bit UNIX workstation(s) (like a
Silicon Graphics Onyx and a matching UNIX server and running one of
the high end CAD packages like UG or IDEAS or Catia. As always
benchmark first!

Regards,