Solidworks performance.

Afternoon,

We are having some major performance problems with the 2D aspect of
Solidworks 2004 sp01.

Problems to date include:

currently not being able to section drawing views at all with the
following error 'There are no drawing views from which a section could
be made' This is really bizarre as it worked fine last week and we
havent changed anything in between.

On occasion when you open and edit a drawing, but close it without
saving as you've changed your mind about what you were doing, it saves
it anyway.

Crashing randomly with the ever helpful error message 'Solidworks has
terminated due to an unhandled error, please contact your local
support representative'

Ghost lines on sectional views.

ridiculously slooooooow performance, that, defying belief, gets yet
slower the longer you use it.

Poor hatching performance.

If anyone can give me any advice I would be greatful as its getting a
bit tedious. I have gone back through all the relevant threads and
cant see anything obvious to try.

Our machine spec is. Dell Precision 340's. Pentium 4. 1.7Mhz.
512meg/ram. Nvidia Quadra graphics card and we're working on
moderately compicated assemblies with upto about 400 components

Rgds
Peter.
Design Engineer.

 

Section views:
in order to section drawing views you must make sure that you have a shadow
box around your drawing view -- this is called activating a view. You can
do this by double clicking the view you wish to contain the section line OR
by right mouse clicking in the view & choosing "lock view focus" -- then run
your section command.

Saving drawings:
Make sure that you do not have the 3d model (part or assembly) open upon
close of the drawing & reopen of the drawing. As even though you have not
actually saved changes the models that were changed actually are still in
memory thus when the drawing is open it will update. Plus make sure that
you do no save any changes to the model as this will update in the drawing
whether you save the drawing or not. If you find that it is still saving in
your situation after checking the above report this to your VAR to have
solidworks fix it -- you may have to send them the drawing with reproducible
steps / instructions to point the problem.

crashing:
Start Solidworks with no document open -- go to tools --options --
performance -- check "Use software open GL" -- close SW & restart the
application. Use as normal for a few days (you may notice some graphical
changes this is normal) + your view rotates may be slower (this is only for
diagnostics). if your crashes seem to disappear then you have now
determined that your video card is the problem. have a look at:
http://www.solidworks.com/pages/services/VideoCardTesting.html to determine
the best video card driver version for your card

Ghost lines:
Make sure your view is not set to draft quality. if setting to draft
quality fixes it then you may want to set it back to draft so that your
drawing is faster & upon print user the "convert to high quality" check box.

Slow performance:
make sure you have a Supported OS : Do NOT USE WINDOWS ME OR 98 !!!
http://www.solidworks.com/pages/services/SystemRequirements.html

make sure you have enough ram by opening your largest assembly & looking at
the Task manager & comparing the actual usage to the physical ram -- if
actual usage is more than physical -- than you need more ram.

Turn off realview graphics!!!! mating is slower in this mode among other
things.

Go to tools Addins & turn off anything you do not need -- only turn on stuff
when you need them

Look under Tools --options -- system tab -- performance & turn off some
things that you may not need to help performance.

do not draw major 2d sketches in drawings -- SW is a 3d modeler not a 2D
sketcher if you need 2D sketcher use AutoCAD & import in SW.

Poor hatching performance:
again, do not draw major 2d sketches in drawings -- SW is a 3d modeler not a
2D sketcher if you need 2D sketcher use AutoCAD & import in SW. upon import
& hatching you may expect this same performance issue with hatching but at
least creating the sketch is easier.

hatching 3d models & faces do not take very long in my experiences. If you
find this in your large assemblies report this to your VAR and or make an
enhancement request.

Hope this info helps.
Steve Tietz

 

Peter,

Join the club!!. SP 1 has totally stuffed drawings - it feels like I am
using SW97 on a P266. One of the worst slowdowns is when you try to move or
resize a drawing view on a GA with multiple secton views.

For the sectioning error - try not to add any constraints to the section
line. I was having the same problem with a section line constrained to the
front plane, I deleted the section, removed the constraint from the section
line and re-created the section and it worked OK.

Hatching - you will probably find that the hatching problem is linked to the
poor performance with section views.

I hung off loading SP1 for a week, and even rang my VAR to confirm that
there were no problems with it before I installed it - all to no avail.
Installing a SW SP is like having a punt on the horses - it kinda wrecks
your faith in SW.

Merry

 

there is an SPR on this. don't know it off hand tho. I think it's still open
tho, and not slated for SP2.0 yet.

Still hoping they fix the display of "offset from surface" cuts problem
fixed in SP2,
nick e.

 

We are having some major performance problems with the 2D aspect of

YEP
I see this as a trend.
I run a SP for the 5 problems I have encountered over the last week of use.
Then the new SP causes 5 new problems I did not have the day before.
IMO
I have used this product since 1997.
It is getting real bloated and difficult to manage. SP 1 is 115mb!
Options prolieferation to increase performance is a sign of poor
performance!
Anyone else sick of detuning the options to get this pig to run?

YEP
Plus I have:
the drawing views that are real slow when you drag them
the feature manager that will not go away after hitting the check mark to
exit the command
the really slow wheel zoom (which is faster if you use the zoom in out tool
button instead)
All this gets somewhat better when you restart the application.

Our machine spec is:
Custom Built 2.4Ghz 1.5Gig ram Nvidia 750xgl
Working on a single part file and drawing
I have been turning off every option I can find that will increase drawing
performance.
The list would take me an hour to retype here
I would send you an email with screen shots if you like
This approach provides only minimal improvements

Wishing I stayed at 2003+
Regards,
Hacksaw

 

This is probably user error. Make sure that the view is activated
before drawing the section lines.

Hmmm. Don't know about that one. Have you tried the "Reload" command
from the drawing? No, of course you haven't, "Reload" isn't available
in the drawing, although it is in the part and assembly. The only thing
I can think of is that people have this propensity to hit "OK" on dialog
boxes without reading them. If you exit from the drw without saving, it
will ask you if you want to save. Accidentally hitting the OK would do
that. Other than that, I don't have any explanation for this, and
haven't seen or heard of it before.

Random, non-repeatable crashes are often attributable to system set up
or software installation. On my website, (http://www.frontiernet.net/
~mlombard/) in the "Rules of Thumb" section, I have a doc on
troubleshooting crashes. There is also a new diagnostic section on the
SW website.

Sometimes following the message instructions to contact the VAR can be
helpful, but that depends on your VAR.

dunno. Is this only when you drag your mouse over something? Are the
ghost lines from a certain feature like a surface feature? Are you sure
the section line is cutting where you want it to? Did you try doing the
cut in the model to see what happens there?

You might try fiddling with your draft/high quality view settings. If
everything is set to high quality, you could save yourself some time by
using draft quality. Also you might try using lightweight settings in
the drawing. Another doc on my website is the Tools/Options settings
for 2004. This identifies which settings affect file size and speed.

If by this you mean that sometimes hatched areas extend into places
where they shouldn't, then yeah, that's a known problem. Aside from
that, could you be more specific? Have you tried using a projected view
with a broken out section?

Anyway, good luck with this, and let us know if anything changes or if
you find something that improves things for you.

matt.

 

Yeah, there are workarounds which effect everyone's time and $$ but this
area of degradation is definitely a problem in SW2004.

The user should not have to fiddle with something which was working fine
or faster in their previous release.
Such as, views not displaying properly or loosing edges or the
appearance of those orthographic views very in line style or look
totally different using the new settings in SW2004.

This workarounds are not productive and SW2004 drawing performance is
not good = negative return on their investment.

BTW, most of you may know this but IronCad use to promote the "Draft"
mode for faster drawing performance and also Inventor adopted this
"Draft" mode... well, neither are fast.... so,... guess what the SW
users get...?? A "Draft" mode!?

Hmm,... could "draft" mode be a user enhancement or marketing want?
"Look, we have a "Draft" mode just like Inventor has!?"

...

 

Yeah, not really, HLR/HLV drawing view was there but, that view display
option did not work properly and was slow (it was a joke and that
interface is not the performance issue we are taking about).

Anyhow, the SW2004 interface is different, using a old marketing name
(Draft quality = faster (NOT!)), works better and is a bit faster than
HLR/HLV drawing view was but...
Overall, at this point in time, there is no real benefit that I see with
this functionality.
My current investment is a loss because the older drawing performance
was/is faster.

"Draft quality" is clearly geared towards large assembly user or not
loading everything into memory (another lightweight thing) or "demand
loading" (I think that is the wording).
Surely, SW users with large assemblies are having issues (I have
problems with single parts) are being told Inventor is faster with large
assemblies and drawings and this "Draft quality" mode is a way of
keeping their users and prospective users interested... = sales.

So if the current interface is slower and they are and have been faster
than Inventor,.. the user interface as well as competing (perception)
with Inventor is a priority, not performance. Marketing wins, the
users loose,.. next release promises... = more sales.

....so, where is my investment is going?? Marketing.

...

 

Cheers for the suggestions chaps, I will see if they make any
difference. the Sectioning is now working, and turning off the show
contents when dragging views seems to have helped.

The only bad thing about posting on here was the fact that in the last
2 days I have had 18 viruses caught on their way into my inbox!!

Rgds
Pete

 

Alway hide in some way your e-mail adress on a NG. Even the _nospam_ is not
sufficient. And 1 post is all these SOB (excuse my French) need to get to
you...