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

Reply to
Loading thread data ...

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.

  1. 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.

Reply to

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"

Reply to
Jerry Steiger

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

"Jerry Steiger" wrote in news: snipped-for-privacy@individual.net...

Reply to

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

Reply to

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.

Reply to

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.

formatting link
formatting link
formatting link
formatting link
formatting link

Reply to

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.

Reply to

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.

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

Reply to

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.

Reply to

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.

Reply to
Jeff Howard

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.

Reply to

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

Reply to

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.

Reply to
Jeff Howard

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.

Reply to

Our company uses SolidEdge and we design and build large automotive transfer and robotic welding systems. The files around here seem to hover between

500-5000 parts. The general consensus is it is SE slow performance wise and has a cumbersome interface. I know they have periodically discussed switching to SW, but the consensus is management will not invest in another CAD program. We recently purchased a single seat of SW just because is so much faster at translations than SE. One of the designers will be sitting at my desk this weekend translating customer files to parasolid so they can have them ready for use in SE Monday morning.

I can't say that SW is any better at large assemblies than SE though. There are all kinds of tricks that have been discussed and shared by others to improve large assembly performance. Unfortunately, some of these tricks require extra time and planning and everyone has to be paddling the boat in the same direction. Easier said than done.


Reply to

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.

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

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

  1. 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.
Reply to

Sorry, this turned out to be an extra long post, most of which is available in user group presentations on my website

formatting link
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.

Reply to

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

Reply to
Jeff Howard

Ok, here's what I tried in 2006 sp1:

I took a file I had, a hex bolt and inserted 50 instances into an assembly, each instance was a difference size configuration.

Then I saved out 50 files copies 1 of each size, and deleted the rest of the configs from the file. Then inserted these 50 files into another assembly.


Opening in lightweight was the same, about a 2-3 seconds. Unchecking lightweight showed that the assy with 50 separate files took about 15 seconds, while the assembly with one file and multi configs, took

5 seconds.

So these results favor the one file, multi config method when fully loading.

Now maybe the results for a file containing a 1000 configs could be different, I just didn't have the time go that far.

If anyone wants the files I used, let me know.


Reply to
Jason Capriotti

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.