Improve Catia performance for Drafting (drawings) 3

[alexlaurenceau]

Any hints and tips on how to improve Catia performance while working in drafting for large assembly drawings?

We have tried "visu mode" and "Do not load ref document" options but when we create the views, Catia loads the files anyway wich cause the computer to crash... (Memory load too high)

We have also tried the CGR or approx view creation without any good results.

Thanks!

Win2k, V5R13


Alex Laurenceau

 

[Configurator]

XP, V5R14

Lee

http://www.lmco.com

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[forfun]

When you tried CGR mode did you first save your assembly as a CGR file and then create a drawing only based off the CGR file? In the past this always worked for us, bad thing is no history.

forfun

 

[alexlaurenceau]

Forfun,
that might be one way but the thing is that we are connected to a database where the files are stored. Ideally, the drawing should be linked to the part with history. I was wondering if there are some little tweaks that I don’t know of that could help.

I know we are not the only one stuck with this problem. Dassault creates the software based on simple part but forgets about performance in a real production environment


Alex Laurenceau

 

[forfun]

Alex,
I agree the drawing should be linked to the assembly/part with history. I question how much effort Dassault puts into enhancing drawings.

Things to try

Go with Configurator's advise, XP, R14

3 gig machine

You might try using a memory manager, this seemed to help us. Catia is a memory hog but does seem to be better in R14.

Open your assembly and delete everything except one small part that has no links. Open a new drawing and create all views needed. Lock all views. Save the drawing but quit the assembly. Restart catia and load the assembly. Hide/show to get the desired results in the drawing, save the assembly and restart catia. Load the drawing and unlock one view, update it, lock it and go on to the next view.

When starting a assembly create the drawing first thing with more than enough views and sections. Creating a drawing of a large assembly seems to be harder than updating it.

Under properties of a view uncheck as many items in the dress-up section as possible.

Keep your tree straight, the fewer sub-assemblies the better.

Do a send-to on your assembly. This will show all the files that are linked to the assembly. When a drawing is being loaded it loads every part and product into memory. We found links going to completely different jobs causing the drawing to load multiple jobs not just the one that was needed.


Back to the CGR's, I am told it is possible to write a program to create new CGR's at night(when ever you want). That way the drawing would never be more than 24 hours out of date. I am not a big fan of CGR's but they seem to be the only cost effective way to create our flowcharts.

Hope this helps, good luck!
forfun

 

[catiajim]

What database are you using? If you are in VPM, then you will have to use something like the CGR Views, as the b-rep method that Eric talks about (I think anyway) is not available yet. If you are in SmarTeam or some other database, it should work.

 

[itsmyjob]

I was talking about the BREP mode which is something between CGR (cache) and Design mode. We have BREP working when you load your assembly (PSN) with cache (you have CGR) then you open the drawing and update a view. The 3D goes in BREP, al least the V5 files (you can check that nothing is visible in noshow).

So the best solution so far is R14SP4, XP, /3gb, BREP.

indocti discant et ament meminisse periti
Eric N.​

 

[Configurator]

Is it 14 or 15 that advertises exact dimensions from CGRs? I think it's 14 (15, I believe, is the release where visualization mode will come from CATParts, not CGRs), but I do mostly RDDs and FTA, so I haven't tried it out.

In terms of memory management, I'd throw out an estimate of about 50% improvement from V5R1-13 to V5R14 (I haven't done any testing myself, so I don't have any empirical data to provide, perhaps someone else does...).

Windows XP with 3 gigs of physical memory and the /3GB switch thrown (like itsmyjob mentioned) is about the best V5 system you can assemble now (I've run a machine with 3 GB and one with 4 GB of physical memory... the 4th gig didn't make a difference). Add the large memory aware switch to V5 (editbin /LARGEADDRESSAWARE c:\Progra~1\Dassau~1\B14\intel_a\code\bin\*.exe) and (visualization/loading settings aside) CATIA will be about as good as it can be from a memory standpoint.

Lee

http://www.lmco.com

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[itsmyjob]

Someone told me that R14 and up should not need the editbin /LARGEADDRESSAWARE

indocti discant et ament meminisse periti
Eric N.​

 

[Configurator]

hmm... I hadn't heard that, but perhaps that was included in the kernel upgrade.

Thanks for the tip. I'll ask the support guys to verify.

Lee

http://www.lmco.com

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[alexlaurenceau]

Thank you all for your reply,
Can anyone confirm that we don't need the /3GB switch in R14? I don't have a 3 or 4 Gig machine to do some tests but it would be nice to know.

Eric,(Salut collegue!)
can you explain some more about the BREP thing? How to activate this? Is that an R14 thing? First time I hear about that.

Forfun,
what does the memory manager do for you? I have seen some giving you a warning when the memory is high but none that I know of can free or purge the memory. Maybe you can suggest one in particular?

Alex Laurenceau

 

[itsmyjob]

Alex,

When you work with cache = ON you have 2 ways to choose from to see the 3D.

Visualization Mode, it is when you have CGR files
Design Mode, it is when you "fully" load 3D files

But another Mode is available only when, starting from CGR files you open the CATDrawing and create or update an exact view. If you look at the status bar you will see that CATIA is loading some info from 3D files... some... not everything.
The 3D spec tree will then expand ONE more level. Do not expand it more it will go into Design mode. So you know when you are in BREP mode when the node expand ONE mode level but you still have nothing in noshow.

The BREP works only with V5 file, V4 will go in design mode when you create / update an exact view.

This is good for memory saving BUT since R14, PSN drawing does not need an update if 3D did not change. The only way you can make that work is, from CGR file, swap to Design Mode and then load CATDrawing.

So it is up to the user to chose between:
working with BREP mode and updating all views everytime you want to work with 2D or
working without having to update views when you load a CATDrawing. So far you can not have both...

indocti discant et ament meminisse periti
Eric N.​

 

[Configurator]

Back to the CGR's, I am told it is possible to write a program to create new CGR's at night(when ever you want).

Indeed. That is a simple task. Just automate DMU cache generation in batch.

Using released cache is a great way to improve opening speed when the cache system is enabled. I'm not sure how well drawings will react to it, though.

Lee

http://www.lmco.com

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[forfun]

Alex,

I do not currently have it loaded, have not had the need in R14, but i believe it was Mem-Turbo 2. With it you could scrub the ram when memory started getting low.

forfun

 

[Configurator]

With it you could scrub the ram when memory started getting low.

How well does that work? Does it make V5 unstable (ie taking things out of memory that should be there)?


I guess what I'm wondering is if you could use it to illeviate the need to restart your CATIA to clear the data in session.

Lee

http://www.lmco.com

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[alexlaurenceau]

How well does that work? Does it make V5 unstable (ie taking things out of memory that should be there)?

That would exactly be my concern... especially if joined with a PLM software like Enovia.

Alex Laurenceau

 

[forfun]

We aren't using Smart Team and nobody was on Enovia at the time. I don't remember it causing any problems. It might cache some parts though, double click on them and they reloaded. The only time we really used it was while loading drawings. In the middle of loading if the memory got too low I would scub the ram and then continue loading the drawing. Command interupts were not as common after loading the memory manager but did still occur. I would think it would still be best to restart catia on a regular basis if on R13. The memory mamager was the only way we could load drawings of large assemblies at that time.

Hope this helps
forfun

 

[Configurator]

^^ But how does it work? Does it only scrub memory sectors that haven't been accessed for a certain amount of time?

What I meant by "making things unstable" was: does it kill cnext (obviously not based on your above description), CatSysDaemon, any necessary .dlls, etc.?

Lee

http://www.lmco.com

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[forfun]

I do not know how it works or how it determines what to scrub, sorry.

To my knowledge it does not make things unstable, however we did still get command interupts but never while scrubing ram.

forfun

 

[Configurator]

Great. Thanks for the info. I might try that out. I hate having to restart CATIA to clear the session.

Lee

http://www.lmco.com

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