drawing enorme

[Spinone]

Good evening to all,
I'm new to the forum and I don't have much experience with sw, so I apologize in advance if my problem will be trivial.

the above problem: the table of a carpentry piece has become gigantic and unmanageable (almost 130mb); It consists of a single sheet containing some views (not more than 5 or 6), details (less than a dozen), cutting distinction and two additional views of the axieme for the indication of welding.

on the net I have not found precise answers to my problem, but I suspect that it is to be searched in the model itself: the part that I go to put on the table is not excessively complicated, but contains within it some dozen "subparts" (in essence screws, bolts and seals) that, in my opinion, weigh considerably the management of the model itself.

advice? similar experiences? errors to avoid?

Thank you in advance who will respond.

greetings

p.s.: the part weighs about 30mb and consists of a hundred functions plus the "subparts" I mentioned earlier, the relative axieme about 20mb; I apologize for the lack of precision but "memory sink", since I have everything on the pc at work.

 

[re_solidworks]

It's hard to give you advice. the import of external elements with "insert part" is not the maximum, nor from the point of view of the performance, nor from the point of view of the management.
to use this mode you may need to enable the option that allows external references in multiple contexts, which opens the doors to total chaos in models with external references.
apart from this you should understand how your part was shaped. Can you tell me + or - how many solid bodies are there? Are there multibody plates in the axieme? as are most bodies (extrusions, structural members, loft/sweep).
I have used a lot of welds lately for carpentry, my models stopped at most to 250 bodies/part and already became rather slow.
the ugliness of this mode is that you can't simplify anything, something quite different than traditional assemblies and when you get to points "without return" are trouble.
the other side of the coin is a great modeling speed if with the massive use of the structural members.

 

[Mike1967]

here we talked about performance and there are many useful tips.

http://www.cad3d.it/forum1/showthread.php?t=18336♪ I don't know ♪

 

[Spinone]

certainly less than a hundred solid bodies; I have extrusions and structural members (I basically have two plates that make up the main body of the piece, reinforced with plates). in addition the holes and screws, dice and or of which I have already said. What seems strange to me is that the situation becomes really unmanageable (work on a workstation of all respect, but at some point it even becomes difficult to place the details on the table at the best).

Thanks for the link, I will take a look.

 

[Spinone]

I read the link, but I didn't find great answers to my dilemma. I want to point out that I have no problems with 3d models: both parts and assemblies are fast and well managed by the system; the problem comes only with drawing (and I just don't understand why the file is so heavy).

from profane I have 2 fundamental doubts:
- references; but I tried with the pack&go to bring everything to the place on my car and I did not benefit any
- modeling with part in part; In essence, I was told to use this technique to promote better management of the final axes (and in fact I never had problems with the models).

 

[Spinone]

to use this mode you may need to enable the option that allows external references in multiple contexts, which opens the doors to total chaos in models with external references.

I honestly don't understand what you're saying, can you clarify?thx

 

[Spinone]

for those interested I solved so (it was a model problem as I suspect):

- the part I worked on was composed of more than 150 functions and solid bodies
- first I have "cleaned" the functions; for example there was a drill made with a single sketch that slowed a lot: I made a single hole and repeated it
- I've eliminated screws and dice on the side, and I've done an axieme
- I updated screws and dice to the current version of sw

now table and models weigh much less (some mb).

Bye!

 

[re_solidworks]

for those interested I solved so (it was a model problem as I suspect):

- the part I worked on was composed of more than 150 functions and solid bodies
- first I have "cleaned" the functions; for example there was a drill made with a single sketch that slowed a lot: I made a single hole and repeated it
- I've eliminated screws and dice on the side, and I've done an axieme
- I updated screws and dice to the current version of sw

now table and models weigh much less (some mb).

Bye!

First of all I thank you for leaving the solution to your problem, it will certainly be useful in the future to others.
As regards performance, there are no great tools available except for a maniacal rationalization of the functions used.
with an open part just go into tools->statistic functions to have a detailed report of the times of reconstruction of each function and every sketch.
at first it is good to check these times to understand what solidworks digests better. just try various alternatives until you find the lightest. In this way, in a short time, you can understand how to model in the best ways for swx.

 

[Spinone]

hi; another problem is that the views remained in bozza quality (probing I disabled some option for automatic passage in high quality). by manually reporting them in high quality the file size has dropped drastically.

I hope it can help someone in the future, bye!

 

[sampom]

hi; another problem is that the views remained in bozza quality (probing I disabled some option for automatic passage in high quality). by manually reporting them in high quality the file size has dropped drastically.

I hope it can help someone in the future, bye!

That's weird. .
Shouldn't it be the opposite? bozza quality = weight and more "light" management?

greetings
Mar

 

[Spinone]

Well, it seemed strange to me, too. I don't know, maybe it's a sw2010 kiss (sp2). If I have some time in the next few days, I'll deepen the matter and inform you.