seemingly using a lot of memory when creating drawing.

[jrochte]

I am using V5R15 and am working with 3d part data that is fairly large(~25Mb). The part data in perticular is that of a steering beam hanger assy in 3D and saved as a V4 model. If your not sure of what ia m talking about , the steering beam is the structure underneath the dashboard of a car. That includes a pipe running from side to side and the frame around the stereo etc...

My job is to draw a rack to hold this part for shi[pping and storing in the automotive plants, 6 to 10 parts per rack. That includes several square tubing etc... that adds maybe 5 6 mb of information. If I rotate/move/instantiate it does fine. Its when I create views in a CATDrawing is where I come into trouble. The CATProduct source file, having 4 instantses of the steering beam, takes several minutes to create three views. Not to mention trying to create 5 views. I then try to save and get a writing to file error or simply get kicked out of the program al;l together. Sometimes I have received a message about all memoory being used.

Now I have checked for viruses,spyware - none fopund. I started up in safe mode to get rid of some unnecessary programs - got a error message about not being able to find licensing - wouldn't let me open program. I simply exited out of programs that were open on my taskbar - no luck.

My system specs:
Dassault systemes certified computer
Dell precision 670 workstation
Intel Xeon em64t processor (with XP 32 bit(autocad does not run in 64 bit))
80 gb harddrive
2 Partitions on one drive
3 gb memory
Quadro fx3400 video card

cache is checked
set at 750 MB
extended language is unchecked

Can anyone help me resolve this? Let me know if there is any other info that will help.
Thanks in advance

 

[solid7]

What SP level?




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[jrochte]

My best guess would be SP1. I didn't download any service packs. Only other way would be if CATIA allows for automatic updates. Do they? I purchased the software the end of june 2005.

 

[solid7]

Is this your company, or are you working for someone else?

It sounds like you have the well-known SP0 memory problem.

If you are your own admin, and assuming that your software is a licensed distribution, you need to get an IBM ID, and get your service packs here:

https://www-304.ibm.com/usrsrvc/account/userservices/jsp/login.jsp?persistPage=true

First, however, you will need to search the IBM page for a reference to your problem, to diagnose the problem and/or obtain a workaround. (type a description in the search bar - the best technical terms to describe - I don't usually have any problems finding them) This will tell you if you have an available workaround, or if you need to upgrde to a service pack or hot fix.

After your first Service Pack arrives, it should come with a "Program Directory." It has all reported bugs listed by Workbench, and SP level. You can take the APAR number, and search for it on the IBM website to find a resolution. ALWAYS check the Program Directory if you have questions relating to bugs.

You can order ANY of the currently supported service packs for Catia.




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[catiajim]

Do you have Cache turned on? If not, turn it on and let CATIA switch the parts into b-rep mode while you are updating the views. That should help memory management significantly.

 

[jrochte]

catiajim,

Yes Cache is on. Never heard of b-rep mode. Do I need to turn it on etc...?

 

[jrochte]

Catiajim,

also, I have not done what solid7 has suggested yet. Just in case it matters.

 

[solid7]

There were a great number of complaints related to memory usage in R15. It was supposed to have been addressed in SP1, but then SP2 came along, and R15 is once again a turd.

If I might give you some GENERAL advice relating to R15, I have found SP1 to be the most stable so far. However, your mileage may vary, so definitely check your program directory for the specifics of your operations.





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[catiajim]

I would do as Solid7 suggests, and download at least SP1 (I think SP3 is out now, but I don't know if it's any good or not).

B-Rep mode is somewhere in-between Visualization Mode and Design Mode. CATIA will use it automatically when you are creating and updating Generative Views. In this mode, the exact Boundary Representation (b-rep) of the part is loaded into memory, but not the entire history of the parts. The only way that you can tell if a part is in b-rep mode is to go to HIDE and see if there is anything there. Expanding the nodes of the parts will automatically switch them to Design Mode.

B-Rep Mode is supposed to take about half of the memory of Design Mode, so you should be able to load more parts than you could with Design Mode, but fewer than you can with Visualization Mode.

 

[jrochte]

CATIAJIM,

Where do I go to HIDE at? Do you mean hide/show? swap visible space? when I do hide/show, the part disappears. If I swap visible space and there is no parts hidden, there is nothing but a green screen. please advise

FYI, I have only taken Intro to modeling which didn't cover most customizing aspects of CATIA. Through my inexperience, I didn't think I would be having these issues.

 

[solid7]

Customizing a user environment is not something that most of us get trained for. I didn't know ANYTHING about it, until I started my own company.

If anyone told you that learning this on your own would be easy, don't ever trust them again. Mark them as deceitful. Much of the experience that is brought to you via this board, comes from users who have worked for some of the largest manufacturing companies in their respective sectors, and many of us ONLY have the experience that we have, because these companies have special agreements and licensing that gives UNLIMITED access to all available functions.

I have spent almost 10 years working for large corporations, and without that experience, (no matter how unrewarding the job was) I would not know half of what I know. I chalk it up to wading in the diversity pool, more than being trained, or using something in a practical context.

Just keep asking, though. You have a large task ahead of you, albeit, not an insurmountable one.




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[jackk]

you said: "cache is on"

have you also set the View Generation Mode to 'CGR' in view properties? (can also preset it in Tools + Options)

When you activated the WORK WITH CACHE mode, did you also turn off the AUTOMATIC SWITCH TO DESIGN MODE?

 

[jrochte]

Jackk
Cache is on. View generation mode was at "exact view". "Automatic switch to design mode" was on. I changed to CGR/auto swirch... is off and no luck. albeit without SP1


What does "automatic switch to design mode" do? If I switch it off, what other things may it affect?

 

[catiajim]

Automatic switch to design mode will do just that. This comes into play mostly in Assembly Design. When you select a part for a constraint, if it is in Visualization Mode, it will be automatically switched to either B-Rep or Design Mode, as required.

If you are in B-Rep Mode, switching to HIDE (yes, I mean "swap visible space") will be empty. If you switch the part to Design Mode, either by right clicking and going to representations or by expanding the tree for the part, then HIDE will be populated.

 

[jackk]

Jrochte:

If the AUTOMATIC SWITCH TO DESIGN MODE is on (active), you're overriding the WORK WITH CACHE setting, and using the design mode instead.

(Cache mode is also called Vizualization mode where you see the light CGR files. When you work with the heavy geometry, you're in Design mode. You have to be in representation or the other)

I'm unaware of any bad affects of turning off the AUTOMATIC SWITCH TO DESIGN MODE, other than having to change the representation if you want to modify the geometry.

 

[catiajim]

No, if the AUTOMATIC SWITCH TO DESIGN MODE is On, parts are loaded in Visualization Mode. They are only switched to Design Mode when you try to do something with them that requires Design Mode (like Constraining, Editing, or Drafting). It's a very good mode to work in when you are working with a large assembly, as only those parts that you need in Design Mode are switched. The rest of your parts are left in Visualization Mode.

Note: This is only true if you are working with CATProducts. See my response to Solid7 in the V$ model into V5R15 thread.