File sizes reduction for DWG/PRT/ASM 1

[CADShark]

Does anybody have suggestions for reducing file sizes of parts, drawings and assemblies in SW? I'm a detail oriented engineer and like to see everything how it's going to be once it's manufactured. That includes true screw and pipe threads. I have one assembly that's close to 100mb and only 50-60 parts.

Thanks,
CADShark

 

[TheTick]

"I'm a detail oriented engineer and like to see everything how it's going to be once it's manufactured. That includes true screw and pipe threads."

What benefit is there to this level of detail? It bogs down the video, eats up memory, and slows regeneration. That, and if your threads aren't lined up turn-for turn, they crash, and it's one more degree of freedom to constrain unnecessarily. It also creates a lot more unnecessary work for the CAD drivers (yourself included), whose time is probably needed for tackling real design issues.

With utmost professional respect, I must say that perhaps an adjustment in your priorities is what is in order.

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[MadMango]

There are a few posts that cover this already.

There's a difference between "detail for detail's sake" and "detail to distribute information". The trick is finding the fine line between the two.

For speed, first get rid of true helix-based threads if you have them. You can also try EcoSqueeze (or UnFrag) to reduce the file size of files.

Ray Reynolds
"There is no reason anyone would want a computer in their home."
Ken Olson, president, chairman and founder of Digital Equipment Corp., 1977
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[CADShark]

Tick,
Thanks for the constructive criticism, but in my line of work, I feel that level of detail is of utmost importance. Cause if things don't line up correctly it could indeed mean someones life on the line. FYI I'm in the medical field. I care not about perfomance nor memory, but the well-being of our customers.

CADShark

 

[SBaugh]

If Detail is that big of a concern, then your not going to able to change the file size. If you do it will not be by very much. There are some 3rd party apps that might help, but it's a "Use at your own risk". See thread559-87953

If you don't need threads then I would highly suggest you get rid of the helixed threads. For an example of faking the threads you can find at my website (located in my signature)

You could up your computer specs (Which you didn't list). Your hardware could be your bottle neck as well.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[CorBlimeyLimey]

CADShark
I sincerely commend you for caring about the well-being of your customers, but how does showing a true thread form help to get things to "line up correctly"?
Also if you "care not about perfomance"then what is this post about?
I agree with The Tick and suggest you use one of SBaugh's alternative thread forms. Annular grooves are probably the best alternative to a "real" thread.

May your customers live long & prosper.

from (the City of) Barrie, Ontario.

OK, so….what's the speed of dark?
faq559-863

 

[CADShark]

SBaugh,
I currently run dual AMD 1900+ athlons w/3gb ram and 256mb oxygen gvx420 vid card. The main reason I create "real" threads is to see where certain fittings will line up at. Majority of our fittings are custom made for us.

CorBlimeyLimey
The post was meant to get suggestion, tips or tricks on reducing the size of the files so I can email them to our vendors. I guess I forgot to mention that, Sorry everyone.

I've come to realize that when I'm designing the equipment it's ok to use real threads but I should then switch over to a representation of them when it comes time to make the drawings.

Perfection is a result of many mistakes.

Thanks a bunch everyone!

 

[EdDanzer]

It will help to make configurations with less detail to reduce file size. The threaded parts should have at least 3 configurations, with threads, cosmetic threads (revolve cut), and no threads. If you use reference planes and axes to mate, changing configurations will not effect the assembly. Many other parts can benefit from configurations, but try to mate with reference planes and axes to eliminate problems with future versions of SolidWorks.
It seems that SolidWorks changes how surface geometry is created in some releases. Any mates using a redefined surface will tend to corrupt after several major releases.

 

[JNR]

So, your special custom fittings are made with the start point of the threads dimensioned to an exact angular location!!!? Do you have problems in drawings with edges disappearing due to geometric interferences between parts? We are in the business of mission critical equipment also, and we would not be killing one person but several hundred at a time. I have been in the 3D CAD business for over 23 years. I can see the occasional use of a true thread form for specific purposes, but to be perfectly honest I think this is a personal problem. You need to recognize emotions for what they are and look long hard and logically at what you are doing. Figure out exactly what you are buying in fact in each case with these true thread forms and eliminate those that do not give you any real benefit. For example. If it is imperitive to have the correct pitch, that does not preclude having rings at the correct pitch instead of complex helixes. Frankly I have a hard time buying your excuses. Sorry to sound so harsh, but I have pretty much seen them all.

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

There are only 10 types of people in the world - those who understand binary and those who don't.

 

[JNR]

BTW: I was not trying to be obnoxious. My apologies. In hindsight, I should have written "personal preference" rather than "personal problem" - gave the wrong impression.

It is difficult to keep our "emotional" side and our logical side separated and understood for what they are. I have been there myself many times, so I am not unsympathetic. Often we have to take a very hard and difficult look at something to finally realize that some of our "must do's" are really not logical "must do's" but our "emotional" justifications for our preferences. In other words we make excuses to ourselves - without even realizing it. It's not an easy thing to do, and I am not taking it lightly. At RCFD we really do have to think about balancing these things, because we can't afford to dump an aircraft full of passengers in the ground but we have to get our design and drafting done in an efficient manner also. Pilots routinely fly manual approaches and land in extremely low visibility (among other things)using an artifically projected image from our equipment - there is no margin for error when the main gear is 20 feet off the deck at 140 knots approach speed.

I think the trick to identifying the exact level of detail required on these things like threads is to look at the exact mating relationships (or degrees of freedom in the problem) and try to limit to only those that are geometrically necessary to achieve the required result. The only alternative is to live with very slow system response time and large files. This also applies to the full/simple configuration trick mentioned by someone else - you can't over simplify either. A dramatic demonstration of this was shown a SW World 1. A simple box containing 120 springs (all the same part number) was demonstrated. Using both a "pretty" and simplfied (bascially a tube) configuration in the spring part the rebuild times were unbelievably different. True, both hardware and SW were slower then, but it is the same principle.

Last thing - I am genuinely intrigued by the issue of how the threads determine where the fittings line up. I assume that you have to determine and control the thread start angle if simplified concentric ring thread models at the right pitch are not adequate. How do you manage to dimension and machine these, and how do you mate them accurately??

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

There are only 10 types of people in the world - those who understand binary and those who don't.

 

[CADShark]

JNR,
Some of our threads are common single point created on a swiss lathe. Those I'm not concerned about. But others are created with what is called a thread mill. I'm sure that in your years of experience that you have heard of this method. But in case you haven't, the bit has many profiles of the exact thread form (pitch, minor dia, major dia, etc...) on it and is normally inserted into CNC. The programmer then tells the mill where to start and how many turns, in a helical path, to take. And just like magic, you have your threads. I must say that not every threaded part we make needs to have this level of detail, but in some cases I find it to be a valuable tool.

Yes, I do realize that I may be overdesigning the parts, and that a simple thread representation my suffice. The real reason I started this thread is because our email server limits us to the size of the files we can send out. Normally I'm sending a few files to our vendors, i.e. parts, drawings and possibly small assemblies. But we are limited to 1.5mb which really stinks. We're a small company and we don't have a T1 or T3 line, we use 2 cable modems at the current time. So our band width is limited.

I didn't want to come across as an anal retentive designer, which is so far from the truth. I appreciate every bit of information that anyone can give me. Im' not set in my ways and I do accept change. Like I had said before, I realize that I need to change my detail styles before I dig myself into a hole of enormous magnitude.

Blair Hollshwandner
Mechanical Designer
Precision Medical, Inc

 

[bobsheets]

I don't know if this will help, but we have done many things to try and reduce file size of component/assemblies to send over the internet. What we found was to use File:Save As: and use the "References" option (lower right). This enables you to save all of the associates parts along with the assembly into another location. We then use .zip to package up the resulting files for emailing. This reduces the .zip file size by 45% approx. over just zipping up the original files. I'm told that doing this removes the "ghost" data from the files. I'm not an IT guy so I accept thier explanation. This is a use of Solidworks functionality that reduces file size. We are not 2004 yet so I don't know if it works there. Good luck.

 

[MElam]

Other tips I've heard for reducing file size for email include covering the entire part with an extruded box or cylinder and name the feature DELETE ME. Addd features that remove edges actually make the file size smaller.

Another one is to suppress the base feature, which should suppress everything and create an "empty" file. The recipient would need instructions to unsuppress in order to see anything.

 

[CADShark]

Yeah I've tried the suppress trick and it did work very well, but like you said (MElam) you have to give a brief instruction on what to do.

 

[JNR]

Cool, I have not heard of anyone using that method of making threads for a long time. Some of your products must be very interesting to work on.

We have had simimlar problems getting file to other people by email. I don't have a file size restriction for received files so I'm lucky and I believe me I appreciate that. Some other ways to go are to use FTP or if you do not need the SW feature data, use Parasolid. I have on occasion manually separated the assembly and part files and zipped them, but it is a pain and you would not want to do it very often. Another trick I have heard of but not tried and tested, is along the some lines as the "Delete Me" trick. You just make a configuration called, say, "dummy" where everything is suppressed and activate that one before you file.

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

There are only 10 types of people in the world - those who understand binary and those who don't.