Large Assembly Advice

Jeez Louise, 11,000 parts in 2400 subassemblies and a lot of in-context stuff? My heart goes out to you. In-context relationships even in relatively small assemblies can slow SolidWorks to a crawl in rebuilds, or even with simple things like editing a mate. I expect that removing the in-context stuff seems out of the question right now, but I think you might be driven to it anyway before you see light at the end of the rebuild tunnel. My advice (seldom followed) is to use in-context relationships (including InPlace mates) ONLY where absolutely necessary to maintain design parameters and ONLY before a design is proven out. All or at least almost all should be entirely removed by the time a design is released for production. If you need help with a logical procedure for doing that I can help you, but it'd be more than a couple of sentences long. Unless you're sorely tempted to do it I don't want to waste the keystrokes, but I've recently gone to the extreme of destroying ALL mates and starting over on a POS assembly somebody else created. After recreating all the mates (takes less time than you might think since you can start from a more logical beginning and proceed very quickly and logically) the asssembly went from about 25 or 30 seconds just to edit a mate to almost instantaneous for the same thing, and from

45 seconds or more for a Ctrl-Q down to about 2 or 3 seconds. And the assembly was much easier to work with (not just faster). Good luck.

'Spork'

Tom Chasteen wrote:

Tom,

I feel your pain. I've been working with 2 large assemblies for over a year and lets simply say I've been less than enlightened. Fortunately, I'm soon going to a company that makes a much smaller product.

But, here's how I've been managing... Multi-sheet drawings must be split up so that each sheet is in a separate file. Child views lying on another sheet are the exception. Sometimes I would make another parent view and hide it. My parts are all imported, so I made sure that all like parts are instanced. Lightweight mode and more lightweight mode. When mating parts get loaded into memory. I made it a habit to 'set resolved parts to lightweight' as often as every minute. In 2004, lightweight assemblies in drawings is a great idea, but there are pros and cons. For detached drawings there are obvious advatages to opening the drawing without the model loaded, but you can't open the assembly lightweight in the detached drawing. For non-detached drawings you can load the model lightweight through the open dialog box and switch back and forth between lightweight and resolved after the drawing is opened. I'm currently having a resource exceeded error message problem with cropping a large assembly view and am tempted to save the drawing as non-detached, load the assembly lightweight and try cropping again. Otherwise, SolidWorks just can't crop the view and I'll have to go back to my cut and paste .jpeg's drawings. I don't like 'rigging' drawing like that, but it's the only workaround I could come up with. Fortunately, after I get all my parts mated in place, I delete the mates and fix them. This is because the design is actually modelled in AutoCAD and documented in SolidWorks.... don't ask, long story. I'd also suggest using the /3GB switch that they talk about in the whats new manual. You may want to talk to your VAR since the MS site seems to be explaining how to set it up on your server or how to implement it into you C++ code. Other than that have fun with all the spare time watching the hourglass. I actually added a second monitor to do some surfing while the views regenerate.

-Jeff

"Tom Chasteen" wrote in message news:Baqcb.3350$ snipped-for-privacy@nwrddc02.gnilink.net...

Here are my "wild" suggestions. Some of these are off the top of my head and may not make sense but maybe I might spawn a good idea so here it goes:

One I would use configurations and have every part have a configuration named simple. This way I could load by that configuration. I am sure you know this one but if you can dumb down a part as much as possible the better off you will be.

I would also possibly use configurations to seperate out the assembly into "zones". Maybe by the way it might be assembled if done in steps. For example if I was modeling a car I might have one configuration that in the engine compartment only and one that is dashboard only.

As for drawings I would use as much of the technology SolidWorks has to speed things up as possible. hide parts and rapid draft will probably be a must if you have any timeline at all.

I hope I helped a little

Ken

Tom,

The advice from Jeff N. covers good ground. I usually try to get 7-10 drawing sheets per file and have found you can generally break a project down to these increments quite sensibly. Also, after you get the whole assy onto sh.1, you can then use subassy's and detail parts for the model and convert to detached drawing, fomerly rapidraft. Like Jeff, I frequently use a parent view that is kept off the sheet to get a better view with less baggage the using part of an unwieldy assy.

Following this method permits assemblies of virtually unlimited size with the possible exception of getting the whole assy on sheet 1 for the ISO view.

Regards,

Dennis

Tom Chasteen wrote:

Wherever possible use driving sketches for as much of your incontext stuff as you can - I normally make a master driving part that only contains a bunch of sketches (eg. plan, & 2 elevations) and a heap of planes & axis hung off the sketches - you can then drop this driving part into many of your major sub assemblies. Driving sketches will also allow you to keep most of your incontext references at the top level, otherwise you can end up with incontext references buried many levels down in the assembly (this will take longer to re-build and some of the really deep references may not update unless you hit ctrl Q a few times.

If you have to hang sketches off other parts use the underlying feature sketch rather than faces/edges/vertices etc. - nothing worse that constantly hunting down 'cherries' when you make a minor change that eliminates a face/edge/etc.

Instead of using section views in drawing of large assemblies you may be better off creating an assembly cut in the model (new configuration of course) and then using this in the drawing - it's heaps quicker.

Beware of cropped views with large assemblies - they can cause major slow down.

Set your SW options wisely (i.e. no auto saves, shadows, etc) - this can all help to speed up the system.

Try to eliminate all 'cherries' otherwise you will find the the entire model re-building every time you hit save (and you must save often).

Note that large assemblies have a bad habit of blowing a fixed price quote because of the huge additional time just waiting for something to happen (drawings, models, renders, etc).

Merry :-)

Phew! you're making my head hurt thinking about this method Merry, but I can see real advantages working this way. I guess you could call this a layout sketch in 3D.

I've gotta try this too!

Thanks for sharing...

Merry's method works well - I've used it on the last two models I've worked on (not a huge number of parts, but lots of splines and intersections through surfaces that gunk up SW) and it has saved a heap of time. Once you have got the hang of what to add to the driving sketches it is pretty intuitive. The other pearl I was given by more than one person on this NG is "Sub assemblies, sub assemblies, sub assemblies......." - couldn't agree more. Another one I use is to use an E-drawing to plan what views I want and which bits to kill to get what I am aiming for - it's also quite handy to use as a reference alongside the drawing - no hopping back and forwards to figure out how one bit relates to the other. Also keeps the customer off your back while you get on with the real drawings! I seem to remember being pointed at Mike Wilson's site ?? which has a load of "collected thoughts" and a good run down on what affects what. Unfortunately I left the copies of the replies at my last place of work. Best of luck Deri

You're probably thinking of Matt Lombard's site. <

>

He has "Large Assemblies" under his "Rules of Thumb" . You might also want to look at "In-context relationships" and "Tools/Options settings".

Jerry Steiger Tripod Data Systems

Thank you everyone for your comments and ideas.

I don't know if I mentioned it, but the incontext stuff is required. I have to (in the end) be able to edit a design table and generate all required drawing and BOMs to manufacture a similar system with different heights, widths, and length of the total system.

That seems to dictate that I can't detach the drawings (part dimensions, hole location, etc. change). However, I will look at detaching drawings for all items which remain constant.

Also, I set up an assembly with a set of planes and one sketch to define all of the variables which I would need to change in the assembly. Something similar to what Merry recommended. I then imported all of the variables into a design table prior to inserting the first assembly. It gave me peace of mind to know that I had control of the environment before having to worry about controlling all of the components.

I then designed and assembled my subassemblies. I would take a sub-subassembly and insert it into the master assembly and work out the incontext mates that were required to get the proper changes. I would then delete the sub-subassembly and continue building the subassembly.

I mate the major subassemblies to planes and then change the appropriate parts to extrude up to or offset from the appropriate plan (sometimes in both directions).

Also, when making the first set of parts, I carefully set up all features (i.e. slots, holes, etc) so that the ones which would not move in relation to some feature or each other were dimensioned so that I could keep their relationships in tact when stretching or shrinking things later.

It took me three tries to really get going.

I'm loading a 15000 parts (12000+ parts & 3000 assemblies) in 90 seconds lightweight.

I mirrored one part and won't do that again. It is a real PITA!

I take the lowest sub assembly that is to be inserted a lot of times and make a fastener assembly (bolt nut and washers) as required to mount the sub assembly and insert the fasteners into the appropriate holes. This allows me to assemble the system with all fasteners included without having to go backwards and insert them in each hole. There are thousands.

Thanks for the cut the assembly idea. I tried one section view and was forced to pull the plug.

I've been doing this with only a gig of ram, but next week I'll be bumped up to 2 gigs. Only the master assembly print (2 pages) with parts bom force the processor to page. I've seen 1.3 gigs commited.

I'll take a look at Matt's site for his tip list. I forgot about that. He always has good advice.

Also, I going to try the 10 drawing limit idea. I may be able to have details, weldments, sub assemblies and major assemblies. I know that with the total assemly on a sheet, I won't be adding many more sheets to that file.

Thanks again to all,

Tom

Tom Chasteen

How do you insert quantites or item numbers on detail drawings for large assemblies?? (Manually???) How do you guys handle that?

Thanks again,

Tom