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assembly size

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spider007

New member
what's the biggest assembly that you can open in catia (or that you succesfully opened.) I have a AMD 64 3500
991MHz, 960mb RAM COMUTER

Right now my folder with all my parts is 118MB big, and i'm not even half way there. The parts are not complicated and running CADUA on the parts woudn't do much good, since the tree only has maybe 10-15 features.
 
Last edited:
Working with big assemblies

To answer your question, Spider, CATIA V5 has no limits for how big parts/assemblies can be. It really depends on your computer, and how much patience you have as the operator.

The question you should ask is: How can I work efficiently with big assemblies?

CATIA has two solutions for you: Cache mode and the DMU Navigator. Both of these use CGR (CATIA Graphic Representation) which are converted CATPart files that are much smaller in size and they make using CATIA much faster. CGRs are tessalations (small triangles) that define the envelope (or skin) of you part and they are only used for viewing (you can measure with CGR also); CGR cannot be edited.

To work with Cache mode: Go to TOOLS + OPTIONS + INFRASTRUCTURE + PRODUCT STRUCTURE and turn on the option to WORK WITH THE CACHE SYSTEM. From now on, everytime you open an assembly of parts, CATIA will load the smaller CGR files, and you'll be able to load many more parts. CATIA will automatically check to see if a CGR exisits and if it is current, and if necessary it will automatically convert the CATPart geometry into it's CGR equivalent.

(it will take longer to open your parts the first time after you turn on WORK WITH CACHE, but it will be much quicker after they are converted)

To view large assemblies: use the DMU NAVIGATOR workbench. All the DMU workbenches work with CGR files to allow you to view, measure, analyze and other things with your assemblies. But you can't create or edit the geometry!

To edit or create new geometry when working with Cache: Use the Part Design, Shape Design or Assembly Design workbenches and open your parts/assemblies. (if you look closely at the tree, you will notice that there are no gray circles in front of the parts - indicating that there is no geometry available to edit.) If you double-click on a part, the CGR version of that part will be replaced with the Geometry version, and you'll be able to work on your part as you have in the past.

If you right-click on your part and choose the REPRESENTATION option, you'll see two modes: Visualization and Design. This is how you can switch back and forth between Design mode (geometry) and Viz mode (CGR). You only have to switch to Design mode for the parts you need to change. And make sure you stay in Design mode until you save the part with it's new geometry.

This is how the big boys (Airbus and Boeing) work with the entire design of their airplanes.
 
hmm, that's defenitly something i'll be playing around with for the next few days.

Probably would have to switch over to the design mode before constraining the part in the assambly.....

Thanks for the info:cool:

ps; my poor atempt was trying to unloading sub-assemblys, but it would load them back up when i reopend the main assambly next time....:(

Chache option seem a lot better.
thanks again
 
spider007 said:
Probably would have to switch over to the design mode before constraining the part in the assambly.....
Click to expand...


You're correct Spider. The parts have to be in Design Mode so the geometry is available to make assembly constraints.
 
Interesting discussion in this topic

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Welcome to the CATIA Forum MeLindaLee :)

The best way to ask questions to the either reply to an existing thread, or start a new thread (about a new topic). That way more people will see your question and more people will help you with answers.

You can also send Private Messages by clicking the persons name.
 
spider007 said:
what's the biggest assembly that you can open in catia (or that you succesfully opened.) I have a AMD 64 3500
991MHz, 960mb RAM COMUTER

Right now my folder with all my parts is 118MB big, and i'm not even half way there. The parts are not complicated and running CADUA on the parts woudn't do much good, since the tree only has maybe 10-15 features.
Click to expand...

;) here's some links to similar posts on improving performance:

Accessing more memory with Windows XP:
Best performance settings > Active Discussions > COE

Another complaint of slow loading:
slow loading > Active Discussions > COE
 
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