SWX 2D Drawing Tips? 1

[MadMango]

I'm wondering if anyone has some good SLDDRW tips for reducing 2d file size. Part of my group is detailing an assembly with 150-200 parts (including hardware). The Assy Drawing is exploded, and has item bubbles, BoM and centerlines for assembly guides.

The 2 sheet drawing is coming in at 9.3gb, and it is taxing the computer's resources. It's a Dell Precision 620 with 1g memory. The natives are getting restless, and they are on the verge of saving the drawing as a .DWG and doing it in AutoCad 2000. They are using SWX2001, SP5.

Thanks all.
"Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[MadMango]

Thanks Scott for taking over this issue with me on the phone. To everyone else, we went over all the common options, and didn't come up with anything new. Does anyone have any experience with SP7 and large assembly drawings? "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[ketd]

Hi All

Most of my designs involve a large number of parts. I have just looked at the statistics for one of them. It is an 8 sheet GA including 4 ISO views 2 plan views section views and BOM's. The original assembly contained 890 Parts (87 unique parts). The drawing file is 12.7 MB.

I do not use Rapiddraft drawing which may effect your performance if you are using them. They are designed to open quicker but do create a much larger file and take longer to create in the first instance.

Beware of splines/helix feature. They can seriously effect the performance of 2D drawings. When I first started drawing with SW I created a true helix spring. Creating a 2D view of a drawing with just 6 spring took over 15 mins to create.

Even for the large assembly above I would not expect to wait for more than 3 mins for a view to be created.

PS I am running a PIII 850Mhz, 768MB Ram, Elsa Gloria II for perfomance guidelines.

I have just installed SP7, but I have not yet created new drawing views at this level.

Regards

Kevin
kevin@ketd.co.uk

 

[MadMango]

Ketd,

Thanks for confirming that some SW drawings can get extremely large. We aren't using RapidDraft either, nor are there any helix features (just sheetmetal parts and hardware and purchsed items). I'm wondering if you manually draw centerlines of exploded parts? Most of our assemblies are tricky to assemble and having these centerlines (as guides) is "almost" a requirement. This is where the down time is coming from. "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[ketd]

MadMango

I do not manually draw Centre Lines.

Regards


Kevin
kevin@ketd.co.uk

 

[SBaugh]

You could have two assembly configurations one with complex parts and the other with less complex parts. Then make your Drawings use the less complex assembly config.

Example: Instead of showing true involutes in your Gears. Show the Gears as just Circles at Max OD.

Hope this helps, Scott Baugh, CSWP
George Koch Sons,LLC
Evansville, IN 47714
sjb@kochllc.com

 

[MadMango]

Good suggestion Scott, I'll pass it along. "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[SnowCrash]

Just tried old faithful "hide views" and "save as" and took a 10 meg drawing file down to 2.5 meg. Without hiding the views it still cuts the file to 5 meg.

Crash 'Try it, you'll like it' Johnson

 

[MadMango]

I had a short discussion with some other SWX users at my company, and we came to an interesting theory about SWX and creating exploded 2D drawings with centerlines that show assembly.

Problem:
1- SWX is a 3D modeler, first and foremost. It wants to live, be happy, and raise it's children in a 3D environment.

2- Creating these massive 2D drawings goes against everything that SWX wants to do. These 2D line segments that are manually drawn in are nothing more than band-aids.

Solution:
Create your exploded assembly model configuration, and insert a 3D Sketch, using the centerlines to show how the parts go together.

Theory:
Once these 3D Sketches are in the assembly, you can now rotate the assembly and the 3D Sketches will also move, saving tons of time in having to redraw all the centerlines in the 2D drawing if you need to show another view for clarity of assembly. When you collapse your assembly, you simply hide the 3D Sketch, since it doesn't change with switches to different configurations.

Roadblock:
These darn 3D Sketches don't show up in the 2D Drawing!

Anyone have any further suggestion? = ) I thought we were on the right track... "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[MadMango]

Nevermind, I'm an idiot... I forgot to go into the 2D drawing (Sheet1/Drawing View1) and Unhide the 3D Sketch. = )

This seems to work rather well now. I'll report back when this is used on a large assembly drawing we have to make (380+ parts). "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[anka]

Hello,
How can I draw a helix? Namely, I'd like to present disorder molecular chains, then their helical conformations, and after that how they pack into helical assemblies?
Thanks in advance.
Regards,
ANITA

 

[SBaugh]

To make a helix:

1) You start a new a sketch
2) In that sketch you make a circle.
3) Close the sketch
4) Pick either helix icon from the curves toolbar or Insert\Curves\Helix
5) You have your choice of the way you can control your helix:

a) Pitch & Revolution
b) Height & Revolution
c) Height & Pitch
d) Spiral

Pitch => is the degree or angle used to control the helix
Revolution=> total # of Revolutions per
Height=> works like pitch except in inches.
Spiral=> a horizontal helix

I hope these are good enought Definitions for you.

And I hope that helps you with your Helix, Scott Baugh, CSWP
George Koch Sons,LLC
Evansville, IN 47714
sjb@kochllc.com

 

[matrix027]

I am a cad designer using solidworks 2001 +
I have a lot of problems with handling drawings.
I dont use cut-views , and i convert them to rapiddraft.
But when i change somthing in the model and i return to load up the drawing , it cost a lot of time.
How can i reduce the size of my drawings (i used also unfrag)


Do u have a solution for me please ?

thanks
michael

 

[RawheadRex]

MadMango,

You're not alone in your frustrations dealing with SW Assy Drawings. Unfortunately, no matter how much we've pissed and moaned at the A.E. from our VAR and the Tech. Marketing representative from SolidWorks who occasionally accompanies him on his regular visits to our company, SolidWorks doesn't seem to get the point that the primary output of the software for a large number of companies (at least in my experience), is 2D DRAWINGS! Although to be fair they have come a long way since I started using SW97Plus.

I understand 100% when you say that your guys are on the verge of exporting to ACAD in order to get the assembly drawings done without all the headaches. In fact I have actually done exactly that before on occasion. I don't know how much time you're losing but I worked on assembly drawings that took nearly an hour just to open up on a workstation with dual P3-850 processors, 1Gb SDRAM, Oxygen GVX1 graphics, running on NT4.

Aside from exporting to ACAD though we've attempted a couple of different things at my company in order to squeeze as much speed out as possible -

1. Similar to exporting to ACAD we've exported jpeg files and bundled them along with exported BOMs into "assembly procedures" (done in MS-Word) and used these in lieu of SW Assy drawings. This can turn into a fair amount of work as well but it can be slightly less painful although clearly at the expense of losing the automation afforded by SolidWorks.

2. I don't know how much hardware that you're using in your assemblies but we've found that minimizing hardware in models can add a significant boost in performance. This is seemingly a no-brainer but I figured it worth mentioning.

3. The other idea that we're exploring currently is liberal use of sub-assemblies/kits with the idea being that smaller sub-assemblies that leverage the automation of SW might go faster. From a manufacturing standpoint this makes out for slightly less intuitive assembly structures (for example hardware that would normally appear in a top level assembly BOM is pushed down to the sub-assembly level where the part count impact is diminished). This might not make sense for your product but we suspect that this will help performance without foresaking SolidWorks automation as we have previously.

4. I saw this mentioned earlier in the thread as well but wanted to repeat it because it is significant. Assembly Section views leech performance incredibly and should be kept at a minimum.

Chris Gervais
Mechanical Designer
American Superconductor

 

[brengine]

My company is going back to AutoCad because of these performance issues. Fancy 3D models mean nothing if you can't get it to paper for the machine/inspection/assemly shops. I really enjoy the 3D modelling world, but the SLOW 2D side and major design intent changes severly increase our design time...To the extent that AutoCad beats SW in getting the job done faster & better for us. I can't believe I just said that but, for us, it is true. :-( We actually stopped creating Exploded views and inserting fasteners, and SW is still not getting the job done anywhere effeciently enough.

Before anyone tones in with the paperless "electronic-age" and CAM systems (that don't need paper), please be prepared to answer how to specify tolerances on produced parts? That is the question we haven't found an answer to yet either.

Then, be ready to answer how the Assembly Shop will put the machine together w/o prints? Some of those guys are not computer proficient enough to navigate around windows, much less the cost of training them all on SW (and the added $$$ for more computers and software licenses out on the shop floor).

Obviously a couple parts here and there will be done on our remaining seat of SW (complex 3D shapes) and converted back to AutoCad to be inserted into our Assembly, but those will only be a couple parts per machine (which could be composed of 100's of parts).

If anyone knows ways around these obstacles I would be glad to hear them, b/c I am not looking forward to going back to soley 2D either.

Ken
bolen.16@osu.edu

 

[Stoker]

Hello Ken,

In spite of SWX's weaknesses with drawing performance, I still find it hard to believe that 2D AutoCAD designs can be more efficient overall. If you take into consideration your entire design process (part creation, assembly mating and drawing creation) is it really true that AutoCAD can outproduce SWX? I can sketch much more quickly and efficiently in AutoCAD, but I definitely cannot design more quickly. I certainly cannot design with more confidence when working in 2D. My products typically contain 500-1500 parts and include a mix of purchased components, plastic parts and sheet metal.

I am in the same situation as you. I am required to produce drawings for all of the individual parts. Assembly drawings are also made which document each assembly step. These assembly drawings are always made using exploded views with explode lines created using the new 2001+ tools. Here is what I do to minimize the slow rebuild times:

1) Work locally as much as possible - working over a network is probably the greatest cause of slow loading and saving times. If at all possible, I strongly recommend working from your local drive. Obviously this gets complicated if you have several different people working on the same project. However, if you can do it working locally instead of over the network will make a HUGE difference in performance.

2) Proper use of subassemblies - you say that you have to show the production people how to put the machine together. I don't know what your product is, but typically most machine assembly situations involve several layers of subassemblies which then all go together into the final assembly. Create the assembly instructions from the subassemblies as much as possible so that you minimize the amount of time which is spent working with a drawing of the entire machine.

3) Proper use of configurations - if you follow step 2, you will be assembling several subassemblies to make up your main assembly, instead of assembling hundreds of individual parts. As a result, when you bring the subassemblies into the main assembly you often don't require all of the detail. So create a configuration in which all non-essential parts are suppressed (not hidden) and use this in the final assembly. The details of how the subassembly was put together are documented in the assembly drawing for that subassembly, but in the main assembly everything that you don't need to supressed.

4) Don't sketch in the drawing - I do not add anything other than notes, dimensions and balloons in the drawing. If there is any 2D sketching to be done I do it in the part/assembly and just show the sketch in the drawing. Sketching in a SWX drawing is just evil. Put any 2D sketches in the part - performance is much better there.

5) Minimize the detail in your parts - this is especially critical for parts which are used repeatedly such as hardware. Make the models as simple as possible - use just enough detail to make things clear but no more. I'm really referring to parts which are purchased where cutting corners on the level of detail in the part won't affect anything.

 

[eranz]

The use of CONFIGURATIONS is the best practice for handling large assemblies (not just in drawings).
You can have a simple configuration of components and simple configurations of the assemblies. It reduces size and resolves much faster. If you have an assembly of 500 components you probably are not intersted in the fillets on some inner bolt.... Yes, it might takes sometimes to create those configurations but it saves you a lot of time at the end of the day!
You can also use advanced select (or advanced Show/Hide) tools to create those configurations or to temporary hide components for quicker drawing views.

 

[RawheadRex]

One of the things that I failed to mention in my post on this subject was something brought up by Stoker. His point cannot be understated! Designing in SW files accessed over a network connection can be and is substantially higher in cost in terms of speed (not to mention lack of productivity which in turn = $).

Unfortunately we're in a situation at my company where we do not have a "proper" PDM solution and pretty much are forced to work exclusively over the network in order to maintain SW models' design integrity. Our "solution" is akin to a running battle with network performance. We continually work with our I.S./network guys who luckily for us understand our (seemingly) insatiable need for bandwith and do everything in their power (which has been surprisingly quite a bit) to squeeze as much speed from our network. The reason I mention this is that I understand that for some people working locally isn't an option but there are sometimes options for increasing performance.

I also liked Stoker's mention of good sub-assembly management being part of the solution to large assembly management. This is also something that can't be understated either.

 

[brengine]

Stoker,
I forget to mention that our AutoCad is no where near "out-of-the-box". We literally have 1,000's of man-hours into VB customization and creating Library Parts. Everything is automated (complete BoM creation/handling, layer management, new part drawing file creation, drawing of basic shapes, material specifiction and common sizes available, our own "Hole Wizard" that works better than SW's, etc...) We hardly ever have to draw a purchased part in AutoCad, and everything in the library has a common handle so we can bring in previously drawn parts all relative to a handle and I get all three views with the parts laying next to each other in correct location and orientation. An example would be a Shock Absorber Assembly, I can drop in a shock, stop, locknut, and mount by just going thru the Library menu routine (for each part) and pasting them at that common handle. In SW I have to find out IF we have each part drawn, CREATE a copy of or DRAW it, CREATE a subassembly, DROP the parts in, then MATE them. In AutoCad I'm done before I even know if a SW part exists.

Granted we do have a PDM that has helped, but it is hard for anything to compete with our existing AutoCad setup.

As far as your statements:
1) PDM copies parts/assemblies to our Hard drive when we open the file. Stays on our hard drive until we decide to put it back on the network.

2) I use TONS of sub-subassemblies(LEVEL 4) in my design. Those sub-subassemblies are usually simple things like shock absorber mount/hardware, bearing block/bearings/spacers, etc... Those sub-subassemblies are put into what we release to the Machine/Assembly Shops as subassemblies(LEVEL 3) and they get one set of prints. Those are composed of usually 5-50 parts. Those subassemblies (usually 2-8) make up the assembly(LEVEL 2). Then the main machine assembly(LEVEL 1) is composed of those assemblies (usually 2-10 of those)

I do all 3D work in the LEVEL 4 and 3 assemblies. Levels 2 and 1 have all of the lower level assemblies mated at the origins so I never have to do anyhting in those larger assemblies except maybe open them to get a relation to another subassembly (say one LEVEL 3 to another LEVEL 3, or possible the LEVEL 2), but we have ways around that as well).

I spend all my 2D time in LEVEL 3 and LEVEL 2. We only do the LEVEL 1 once, if we can help it.

3) Haven't tried configurations were parts are hidden. I'll have to look into that, but I guess I'm not sure where to draw the line (what I need to see at those higher levels and what I don't).

4) Drawings only contain notes, dimensions, balloons, and BoM. We gave up sketching in there long ago. We do any necessary sketches in the part file too.

5) We DO minimize detail in purchased parts as much as possible. But taking detail out of manufactured parts leads to interferences, unless user remembers all fillets/cutouts that are "hidden" in that configuration, so that is a user choice there. I like the idea, but envision myself (if I remember hidden features exist) constantly opening those parts, unhiding the detail to check it's size/radius, hiding it again, then going back to my assembly to do whatever I was trying to do to the mating part in the first place.

We don't put any fastener hardware in anymore, and the Assembly guys are pretty p.o.'d about that, as well as the possibility that it can lead to design interferences as well. Some designers put in a BLANK part called "1/4-20 X 1in long.SLDPRT" (with no mates, or FIXED) just to get the BoM right, but if something changes they usually forget to go thru and update these files, so the BoM is wrong again.


Stoker and Eranz,
I will look into creating more configurations were I can hide uncritical parts, but again I have to figure out WHAT is uncritical and WHERE?

Thanks for all your input, I really appreciate it. Anything I do in SW now is on my own time, but I DO want to find a way to make it work. If we had ANY bare-bones 2D package, then SW would win hands down. But to be honest I think it's too late for SW at our company.

Again thanks, and PLEASE post any other ideas you may have about this in the future.
Ken

 

[brengine]

Stoker,
I missed a couple of your points:

"These assembly drawings are always made using exploded views with explode lines created using the new 2001+ tools."
-->I didn't know about this I will look into it, but since we stopped making Exploded Views in SW b/c of the time involved, it is probably a mute point.

"I can sketch much more quickly and efficiently in AutoCAD, but I definitely cannot design more quickly. I certainly cannot design with more confidence when working in 2D."
-->Yes and no. What do you do if there's a major change in Design Intent? How far down do those changes propigate? If a part size or feature location changes then a Parametric Design is great, but what if you want to add a part in the middle of a big jumble of parts in you assembly OR you/your manager decides to use a lift instead of a pick-and-place? How many Mates and Relations have to broken and how many more created in their place? Thats the real Design Time loss we see...Changes in Design Intent in a 3D Assembly take much more time to change than in 2D.

Just some more of our roadblocks. Thanks again for the input,
Ken