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ProE Vs Catia..

james.lynch

New member
People,


I would like to know if anybody out there is currently using both Catia and ProE.


I would like to know the advantages and disadvantages and also about functionality,specifically surfacing.


which is more popular in industry and why? I will be finishing my masters this year and will be looking for a job would like to know is Catia worth learning?


From a ProE users point of view, how difficult is it to learn?


I have done a search on this and found a post over a year and a half old which doesn't really answer my questions.


I'm talking about WF 2.0 and Catia V5R14 and above..


Thanks,


James
 

Israr

Active member
ProE is good in large assembly structure, Catia is good in surfacing.


Catia has an added advantage of direct Catia ABAQUS interface.


ProE has interface with ADAMS through Mech/Pro (and now an interface only version is also available) while having its own MDO.


Catia has direct interface with LMS virtual Lab while having its own mechanism modules,


ProE has an added advantage of superior BMX module.


What I have heard of Wildfire 3.0, will be much ahead of Catia 5R15.


Israr
 

james.lynch

New member
Israr, Thanks for the Reply, very informative.


Re. Surfacing, is it surface creation methods better or is the surface definition mathematically better? anybody know the specifics of this?


Thanks, and if anybody has any other coments to add,especillyabout how steep the learnign curve would be for a proE user, I would be greatful.


James
 

Israr

Active member
Surfacing is vast in Catia than ProE, I mean lots of controls and options than ProE.


The learning curve is interesting. It was steep for ProE till 2001 than Catia V5 but now Wildfire 2.0 is really easy, and honestly speaking has paralleled Catia v5R14, rather I would say is easier.


I would be happy to hear from others too.


Israr
 

pedja666

New member
Surfacing is really deeper in Catia but that has disadvantages as well. There is Cataia 5 a powerful freeform surfacing modulus which is useless because it is completely unparametric except maybe for the earliest concept stage in ID.<?:namespace prefix = o ns = "urn:schemas-microsoft-com:eek:ffice:eek:ffice" />


I would like to underline something else as the main difference: Top-Down Design.ProE is years ahead of CATIA 5 in this department.


The second difference is the concept of incorporating the surfacing into solid and final geometry. Catia hasa very strange concept of so called open bodies and solid bodies having separated completely surface and solid geometry. This can be quiet confusing because the feature history is completely separate so it is very difficult to follow the model creation logic.
 

Isair

New member
From I knows Pro/E is much stable, and needs Les hardware then CATIA (I'm talking about WildFire 2.0). Then how much often do you use surface modeling unless if you working in automobile, airplane industry or with plastic parts. Further NC and manufacturing, ProMechanica are better in Pro/E. My opinion is that is good to know other software but I will take expert in Pro/E and know rudiments of CATIA.
 

SixthChameleon

New member
Having used CATIA V5 on a daily basis alongside Pro/E for the past six months and giving it the benefit of the doubt for that period, I can say unequivocally that on the basis of capabilities, stability, and performance, Pro/E is superior. In many cases, there is no way to compare the two platforms on a feature-to-feature basis because for many of the features of Pro/E, there is nothing comparable in CATIA. Here is a short list in no particular order:


1. Family tables: There are no family tables or any feature that goes by another name that is analogous in CATIA. CATIA has something called design tables which allow the part to be regenerated, or "updated" in CATIA parlance, with different dimensional values (AFAIK there is no ability to exclude features from within the table). The table does not control the geometry of multiple parts though. If you want to update or add a parameter to all the parts in a hardware library, you have to edit each individual part. It would probably be possible to write a macro to do such a thing, but why?


2. Patterns: There are three kinds of planar patterns in CATIA: rectangular, circular, and user patterns. There are no pattern tables. The first two should be obvious. The latter allows a feature to be patterned randomly based on a sketch containing points, e.g. a feature is placed at each point in the sketch. There is no way to pattern in three dimensions, whereas conversely Pro/E has the ability to generate patterns with up to six degrees of freedom. Also, Pro/E patterns are generated adaptively, whereas pattern members in CATIA are merely copies of the original geometry. If you were to pattern up to a convoluted surface in Pro/E, each pattern member would terminate where it intersected the surface. In CATIA, each pattern member would be an identical copy of the original, some instances would protrude through the surface while others would stop short.


3. Simplified Reps: There is no memory management in CATIA. There is a feature called "Scenes", which allows you to explode components as well as hide/show them, and call up the state at a later time, but there is not way to show an alternate or less memory intensive representation.


4. Layers: CATIA has layers, but they don't work. You're stuck with hide/show.


5. Units: CATIA can only work with one set of units at a time. The unit system is entirely session based.


6. Drawing views cannot be re-tasked. Once a view is created, there is no way to change its type or reorient it.


7. Smart BOMs: With CATIA, you can configure a bill of materials in product mode and then automatically generate a table and balloons in the drawing. The table and balloons are not associative, however. The balloons, when generated, all appear in one view, but they're "dumb". If you want to reorder the item numbers, or make any other change, you must re-configure the BOM in the product and then show a new table and balloons, which makes it basically useless.


8. Etc... I could go on, but I don't have the time.


There are serious performance issues with CATIA V5. The implementation team at my company has created benchmarks to compare the performance of CATIA and Pro/E. The benchmark is executed on the same hardware platform in both instances and analyzes equivalent large assembly models and drawings of both tools, comparing retrieval, regeneration times, drawing performance, and graphical performance. To sum up the results, the benchmark takes 4.5 times longer to execute in CATIA compared to Pro/E. We're still using Pro/E 2001, so any performance gains realized in Wildfire 2.0 will only increase the margin.


One of the workarounds implemented at my company to deal with the performance issues is to create separate files for each drawing sheet on top level drawings. Otherwise, CATIA experiences memor overflow problems and tends to crash, orin Dassault's preferred terminology, CATIA experiences a "premature exit".


CATIA V5R1 was released more than six years ago, and is currently at R14, so clearly the performance issues are not a matter of "software maturity". I believe there are some fundamental flaws in the V5 modeling kernel which Dassault has found insurmountable. Our application engineers have been told that many of our enhancement requests cannot or will not be implemented in V5 and that V6 is currently in development (Dassault will deny this of course). I believe that one of the flaws involves the way that V5 handles assembly components. There are indications that components are essentially linked copies. When a sketch, for instance, is edited in the assembly, the sketches for each instance are displayed at once. It then takes an inordinate amount of time to update the feature(s). Even if the component is edited in a separate window, the performance remains the same. Mass properties reports take a long time to generate. For example, a medium sized assembly can take more than half an hour. Standard procedure at my company regarding mass properties analysis is to perform it overnight. Also, in support of my "linked copies" theory for assembly components, on several occasions I have seen different masses listed for separate instances of the same component in an assembly mass properties report!


I have written a rather scathing report, highlighting many of the negative aspects of V5. There are also many things which V5 does well. For instance, it has a very easy-to-use and convenient interface. In balance though, when compared to Pro/ENGINEER, it comes up short even when compared with old versions.
 

dlongmi

New member
SixthC,


To further bolster yoursuspicion that V5 has an inherent kernal issue, rumor has it that after Paine(sp?) sold Solidworks to Daussalt he informed them of that very fact. Again...RUMORS have been floating around the watercooler for a long time thatwhileDassault was scavenging what they could from Solidworks for V5 the "deficiencies" became apparent. When pressed, Paine(sp?) admitted the issues.However, he still walked from the deal with 380 million large. Not bad for "stealing" Pro/E, eh?


V5 is essentially reworked and bandagedSolidworks with "Frenchness" added. The basic flaw purportedly still exists and from Rumor Control Central it always will.
 

dr_eng_x

New member
Where is the ProE interface with ADAMS?


Personally, I find MSC products hardly user friendly though I have not heard about a powerful program as ADAMS I do not find other than MSC.ADAMS If only there'sa workbench or integrated user interface...unless there's another ADAMS


Israr said:
ProE is good in large assembly structure, Catia is good in surfacing.


Catia has an added advantage of direct Catia ABAQUS interface.


ProE has interface with ADAMS through Mech/Pro (and now an interface only version is also available) while having its own MDO.


Catia has direct interface with LMS virtual Lab while having its own mechanism modules,


ProE has an added advantage of superior BMX module.


What I have heard of Wildfire 3.0, will be much ahead of Catia 5R15.


Israr
 

proengineertips

New member
wow.. indeed



What I can say it depend on the industry you are in.



If you are going into automotive, I'ld recomend CATIA. CATIA has very
good free form surface control. It can create good and easy
surface continuity.



If you are doing electronic product design, I'ld prefer Pro/E because
it is parametric. create and modification is easier and faster in Pro/E.
 

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