Hybrid design enabled Vs disabled - With geometric set ON in both the conditions 3

[namelessudhay]

Hi,
In Catia V5 R20, I get options to enable or disable hybrid design. With that I also have a choice to create a geometric set or not. My question now is this:
What difference does it make between Hybrid design enabled and disabled but keeping geometric set on in both the conditions?

I read few forums about hybrid design, but this specific combination is not discussed in detail. For me, when I did few trials in Catia, I didn't find any difference either. Pl. help. Thanks.

 

[sudhakarn]

Hi,
In hybrid design both solid and surface geometries are created inside the part body ( if the body option is set to on ). If you turn off hybrid design surface and wireframe geometries are created in the geo set. Hope it helps.


Sudhakar.

 

[JeniaL]

don't use hybrid design. use ordered geometrical sets or usual geometrical sets. this will help to better organize and understand for others spec tree.

 

[namelessudhay]

Thanks SuDhakaran and Tikito. But my question is little more specific. What I observe is that there is no difference between hybrid and non hybrid, if the geometric set is turned on. Can you clarify pl.?

 

[jackk]

Nameless,

You asked: My question now is this: What difference does it make between Hybrid design enabled and disabled but keeping geometric set on in both the conditions?

It makes no difference. CATIA still behaves the same in either mode.


Tikito,

I have to disagree with your suggestion. Many users prefer Hybrid Design where all the geometry is found in one place (Part Body). It really depends on the company standards, and having everyone working the same so all CATIA files are easily understood (as you said) and modified.

 

[JeniaL]

the difference is if hybrid design is enabled open bodies can be stored under part body.

Jackk you are right it depends on company standards. i'm into aerospace and have never seen aerospace companies using hybrid design.

 

[namelessudhay]

Thanks, Jackk. Just out of curiosity, why does catia have such two options, when there is no functional difference?

 

[jackk]

Originally, CATIA V5 was non-Hybrid, and most users learned (and still prefer) that method. Hybrid mode was added much later (release 17?) at the request of a new company who was converting to CATIA V5. It was added as an option, so companies could choose the method they preferred. Most user companies choose not to change the method, since their users were very familiar with the original, non-Hybrid mode.

 

[Albigger]

Tikito,

Can you post a screenshot of a typical tree you might see? We use hybrid design but more because that's what we learned (also aerospace) so I'm curious to see.

Also - if we disable hybrid design, what will happen when we open a file that was made with hybrid design enabled?

 

[JeniaL]

take a look. the spec tree is clear and easy understandable even for a person who have never worked on this project.

 

[ferdo]

Hi

Different opinions

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[jackk]

Albigger asked: "if we disable hybrid design, what will happen when we open a file that was made with hybrid design enabled?"

You will be able to open and edit and save the model. You will notice that all the Hybrid bodies will have yellow gear icons, instead of green. As you edit the model, you will probably notice that somethings behave a little differently (never found a definitive list) but your model will be fine.

If you add a new body, it will have a green icon.

Here's a good description of the icon colors:

http://www.eng-tips.com/viewthread.cfm?qid=145619

 

[lardman363]

I believe the only thing the geometrical set setting does is if it is on, when a new part is created, it will create a geoset. If it is off a geoset will not be created when a new part is created.