how is Pro-e comparing to other softwares

[skwasim_smile]

hiiiii


I just wanna know how is pro-e comparing to other softwares like Catia,SolidWorks,Ideas etc... i have worked on all these softwares but not the full extent so if u guys anyone out there have a detail info plz let me know the advantages n disadvantages of pro-e over others


Thanx in advance

 

[AHA-D]

ProE (most 2001, bit of WF2) versus Solid Edge (V15)


Present in ProE, lacking in SE :
<UL>
<LI>perimeter command allowing construction of 'flexible' complex geometry</LI>
<LI>analysis tool results can be used in relations and parameters</LI>
<LI>access to part features and dimensions directly in assembly environment through expanded model tree</LI>
<LI>presence of 'higher order' features like varying helical sweep</LI>
<LI>conversion tools from part to sheetmetal (e.g. hollow box to folded box by indicating regions to rip)</LI>[/list]


Present in SE, lacking in ProE
<UL>
<LI>file properties conforming to Win, making them accessible from outside CAD</LI>
<LI>ad-hoc associative part copies in all environments as base model, construction or boolean operator</LI>
<LI>any file used anywhere 'remembers' it's disk and folder location</LI>
<LI>hardly any necessary tools outside basic package</LI>
<LI>part transfer through assemblies and subassemblies, keeping relations</LI>[/list]


Although ProE is more powerfull when you add all functions (be it that the gap is closing rapidly) the overall impression (after one year of full time ProE) for me is that I wouldn't trade SE for a dozen ProE's. Any comparable function is at least twice as fast accomplished in SE, the interface is streamlined and intuitive, something only starting to emerge in WF. This goes for part modeling, assembly, draft, assembly, weldment (is there such a thing in ProE ?).


SE is also more robust when changes are applied. The basic reason is ProE being pinned down on the 'zero degrees of freedom' idea, while SE can live with both under- and overconstrained conditions, and has a 'forgiving' nature. Lost references in ProE throw you into resolve mode hell, SE shows you that something's missing but happily proceeds when a solution is possible. Same for assembly : throwing out the first part keeps the assembly alive, although obviously the next part in line will be lacking references.


There are lots more instances where I find SE is less labour intensive and far more existing work can be saved and re-used, the list would be to long to write here.


So yes, I can work with ProE but I'm always happy to come home to SE.


Alex

 

[mgnt8]

"Same for assembly : throwing out the first part keeps the assembly alive, although obviously the next part in line will be lacking references."


Tryfreeze_failed_assy_comp and you'll be that much closer to home. As far as Pro/E not being "robust" when changes are made, some would argue Pro/E models will be as robust as anything else as long you know how to create features correctly. I guess someindustries demand a bit more care & attention to detail than solid edge userswould provide.

 

[marks]

Ouch...

I've been using solidworks for 7 years, ProE for 3 (2001, WF, WF2). For 99% of the work I do I would choose solidworks over ProE for the reasons listed by AHA-D. (Medical device industry.) For quick exploratory design work (i.e., designing several differentconcepts or iterations)solidworks runs circles around ProE. Of course, you can design poor products in any cad system. Our company is in the process of moving from WF2 to solidworks.

 

[Dell_Boy]

I had the misfortune to be using Solidedge for a few months and would
never want to go back there because of several huge gaps in it's
functionality.





The ones that really stick in my mind are



The whole system for families of parts is far more limited than
SolidWorks
and a joke in comparison to Pro/E. You can only edit the values of one
instance at a time in the table, each instance MUST have it's own file
and the instances in assembly mode are unmodifiable blobs.



Assembly family table were effectively only added in v16. Previous
versions capabilities in this area are are so limited they are not
worth mentioning. Interchange assemblies don't exist and SE family of assembly files are truly huge in comparison to Pro/E



Pro E users know to reference to faces and not edges of bodies where
possible because of the child problems that you are likely to run into with
chamfers and rounds. With SE you can only reference edges.



There are too many other gripes to list here.





Also tried SolidWorks for a few months and found less limitations than
SolidEdge however in the line of work I am currently in my biggest
problem with Solidworks are limited patterning options with respect to
Pro/E and it doesn't handle large assemblies well.



Our top-level assemblies are typically 3,000 - 10,000 parts. Not large
by world standards but more than enough to make Solidworks sweat and be
awkward to work with.



The family table editor is not wonderful, particularly with large
families and I find the relations editor much more difficult to use.



I also think Intent Manager in Pro/E sketcher runs rings around both SE and SW sketching.



Assembly files remembering full paths in SW and SE is a right pain when
you want to promote items to the library. In a suitably configured
Pro/E system, this lack of path memory should
not be a problem at all, even without Pro/PDM, Intralink or Windchill.




Though the search path and library catalog take more effort to
configure they allow possibilies that SE and SW do not such as
retrieval of components by simply typing the model name.



DB






BTW It seems that neither SW or SE allow the first view of a drawing to be a X-section



Edited by: Dell_Boy

 

[AHA-D]

If I would have been working with ProE for only a few months I probably would've considered it unfit for the job. Meaning that if you don't take the time to adapt yourself to a way of thinking and working you can only end up in frustration.


That was exactly my feeling with ProE (2001) the first months. I couldn't pattern anything because I wasn't used to be forced to build a feature with the patterning parameters already included. I also struggled much to often with ProE not being "smart" enough to "understand" that for instance I really needed 270

 

[XICANDER]

Try to do a mapkey. In SE V15, it had to be done in VBasic, isn

 

[Dell_Boy]

Yep,



rotational patterns are fun to learn but once the technique is mastered you will wonder why you ever had a problem.



Sketcher is easier to control once you learn to sketch out of
proportion. It doesn't matter as all will come right when the
dimensions are finalised. If you get equal lengths popping up, either
disable them in constraint manager or better still ignore them as they
will disappear once you apply the dimensioning scheme you want.



If you are accidentally picking end points, there is a good chance that some of your segments are sketched too small.



You wouldn't have two different parts in your system with the same part
number, why do you have two files or instances with the same name? With
over 10,000 different components modelled we have no duplicate names
ANYWHERE. You also appear not to have fully grasped the concept of
working folders and search paths.



With assemblies containing lots of components assembled concentrically
on shafts, eg. spacers, bushes, internal circlips, bearings, lock
washers, keys etc. external views are almost useless for showing how
they are assembled, whereas a single sectional view is usually enough.



SolidEdge and SolidWorks will never catch up to Pro/E because
Unigraphics and Dassault Systems also have their high-end packages NX
and CATIA. As long as they have two products, they have to leave
functionality out of the mid-range software to justify the price of the
high end.







DB



Edited by: Dell_Boy

 

[AHA-D]

Off topic, but still ...


The old part-number/filename discussion.


I guess it will never be solved, as it depends a lot on what you're doing.


Of course each component needs it's own unique identity, the only question is whether it should be reflected in the filename or not.


If you're purely assembling existing things then there's nothing keeping you from having the "partnumber equals filename" scheme. As soon as you're designing and creating on the fly problems pop up. Unless you have absolute authority you're probably not allowed to enter partnumbers on the fly. Meaning you're creating some arbitrary name while designing and will change it when everything is production ready. Renaming in parametrically linked business is always a tricky business. If it's only assembly and drawings then things can still be feasible but when interpart relations, assembly relations and tables are also involved it's easy to create havoc. When the part number is just a property (parameter) of the part file then even the people at logistics can do this job without knowing how the design was made. Descriptive filenames are also easier for humans, albeit that I still remember what the 500-or-so uPVC profiles from my past life were named and looked like.


So from a designers point of view I don't agree with filenames needing to be unique, as long as they make sense in the context. You don't have any problem either to understand that the 'James Brown' coming to sell you nuts and bolts isn't the same as the one that is mentioned on the radio, do you ?


Alex

 

[skwasim_smile]

thanx guys for the response i really appreciate ur concern towards this topic hope u guys keep this discussion going on with more intresting stuff


thanx