boolean operation 1

[par1]

I'm trying to assemble two different bodies & getting follwing message:

"You are trying to create boolean operation which breaks relation order between geometrical elements. Operand body will not be moved under the boolean feature, Do you want to continue?"

What action should I take?

 

[solid7]

Are you using hybrid design?

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[catiajim]

I would try the first. If that doesn't give you what you want, then hit undo and try the second.

As Solid7 mentioned, I suspect you are using Hybrid Design. Turn it OFF and recreate your part and I think you will be happier.

 

[par1]

As you know, When we start new part, we get 3 options,
(1) enable hybrid design
(2) Create a geometrical set
(3) Create an ordered geometrical set

So which option I need to click when starting new part,
(my part is hollow one with few ribs)

I don't see any problem right away by clicking "yes" but does anyone know like while release procees or any other issue will create later on?

 

[catiajim]

This has been discussed and debated several times. Search the forums for Hybrid Design and you will find a lot of information.

 

[solid7]

I don't see any problem right away by clicking "yes"

On the contrary - it looks to me like you've already found one of the biggest problems with using hybrid design.

As Jim said, though, it's a re-hashed topic. You would be better served by searching than asking again.

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[par1]

Basically, I do have HD2, catia v5 R16 license & novice user. I tried to read the past reply @ hybrid desgin
& learned that when we use surface (open bodies) & solid together, assuming class A surface people will need more.

on my system,

The default clicked option is - Enable hybrid design,
Non clicked option is
(2) Create a geometrical set
(3) Create an ordered geometrical set

I'm making solid part with a few bodies & using GSD for plane interaction with solid body.

My customer doesn't accept hybrid bodies & I already finished modeling so do I need to make the model again?
or any option to convert into non hybrid version?
Hope, if someone can help !

 

[solid7]

My customer doesn't accept hybrid bodies & I already finished modeling so do I need to make the model again?

Yes, you do.

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[par1]

That's the quick reply but to avoid next time any big mistakes, I will appreciate if you can reply few more ans,

(A) Which option you want me to choose out of three?
(1)Enable hybrid design,
(2) Create a geometrical set
(3) Create an ordered geometrical set

(B) Is any way to find if the given model is hybrid version or not like by looking properties?
(C) Can I use GSD next time or not at all?

 

[itsmyjob]

You should define in your CATIA environment the option, so you won't make the mistake again.

I suggest you:

DO NOT use Hybrid Desing, as you client does not accept it.
DO NOT use OGS, as it reacts like Hybrid Desing.

Use Geometrical Set for Surfaces.

You can also ask your custumer to confirm your choice.

GSD might be enough, ask your CATIA business Partner a demo on Free Style to understand what it can bring to you.

Have fun

Eric N.
indocti discant et ament meminisse periti ​

 

[jimicatia]

Just make sure that your working environment is set to standart(Non-hybrid) design mode.

from tool> options> infrastructure> part infrastructure

uncheck the Enable hyrid design option.

and you do need to change this option untill you want to change your design environment.

so next time, when you open a new part file, just click ok.
create a geometrical set option is optional, depending your needs.
and create an ordered geometrical set option is only for hybrid design.
I hope this helps..

 

[jimicatia]

correction for my previous posting

and you do not need to change this option untill you want to change your design environment

 

[par1]

Thnks for reply,

Just one more question wanted to raise related to my previous model (enabled hybrid design)
& the the one that i will be making new one for the same model(without hybrid design or with geomtric set).

Actually, I will be end up doing the same operation like boolean operation to have the thickness & volume measurement. (Not the shell) Also, GSD intersect for making ribs,

so only intial click would be different while starting new part & everything else is same?

 

[catiajim]

Pretty much. There is some differences in behavior between Hybrid Design and Non-Hybrid Design - starting with the fact that the wireframe elements will be in a Geometric Set. Non-Hybrid Design is the way that CATIA has worked forever. In it, the wireframe features are not order dependent and they are reusable whenever desired.

 

[Stargazer81]

Why is everybody complaining on hybrid design? I always have it enabled (love it) and my boolean operations works perfect. (Exept in R14 whitch seems to have problems when using booleans, R16 works just fine.)

Personally I don't think that you should use these operations unless it really makes the modelling easier.
But if you're not sure of exactly what you are doing, you can really mess up the model by using to many bodies.

I guess that many have these problems because of the use of old start models with a non-hybrid partbody, and then you cannot add a hybrid body to this.

 

[solid7]

Why is everybody complaining on hybrid design?

Because it's overly burdensome. Pure and simple. Most companies don't accept hybrid design, and won't take the data. And, hybrid models are not compatible with many processes. If it is compatible, it is NOT interchangeable. (it has to be all or nothing)

My biggest complaint is the very fact that they included it - seemingly to make UG, Pro/E, and Solidworks users more comfortable. (with a product that is none of the above) If you had ever received data in hybrid mode, and actually needed to work with that data in the "conventional" format, you'd complain, too.

Hybrid design. What a hassle! Instead of wasting time/money on that, it would have been better spent developing/purchasing 3D text capability, and including STEP translator in every license. (like most other CAD systems)

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[catiajim]

But if you're not sure of exactly what you are doing, you can really mess up the model by using to many bodies

I have over 3,000 users here. The amount of confusion that Hybrid Design will cause with the users who are used to V4 (and V5 pre-hybrid design) would completely overwhelm our support staff, and more than make up for any benefit that the few users who understand it would ever hope to have.

 

[Stargazer81]

Of course I understand that this new to all to the ones that used V5 before hybrid design was available. But most of the "experts" I have spoken to can't say that they know what hybrid design really is. I think it's obvious that you should be able to add a plane/point/surface directly after a feature in a body. Otherwise you will break the "time-line" that you need to follow from top to bottom in your tree (to avoid update cycle problems). How do you know after witch feature a surface or plane is if Catia forces them to be placed in an geometrical set..?

I don't like that some companies just forbids ways of working. If I can make my models and all the changes needed 5-10 times than the designers that tells me I'm wrong (or works in some to me mysterious V4-style method), who is right?

Also have to admit that I'm a former Pro/E user so i guess it's the biggest reason to why i think this is the "right" way. Also love this discussion..

 

[catiajim]

That would be fine if you were the only person to ever revise that part in the future. But what happens 2 years from now, when you have moved to a different program or company, and now someone needs to edit that part? If you don't model your parts per our standards, then it will be much more likely that we have to re-model your part rather than edit it.

In traditional CATIA modeling, you can at any time investigate the parent/children of any feature of the part. This helps you rapidly identify which components are used by your feature.

 

[solid7]

Stargazer81 - Catiajim said it well enough, but ALL of your statements could be turned on their head by this admission alone:

Also have to admit that I'm a former Pro/E user

You are what I like to call "tainted". That's when you bring YOUR bias for another CAD system, and try to influence the others, just as you feel is being done.

Hybrid design was an afterthought. I am QUITE familiar with what it is, and can tell you with no second thought that I believe 100% that it is NOT better. It was Catia's attempt to put themselves on the same train of logic with the other software companies. Again, in my opinion, that was a concession, a step backwards, and an impedement to a very innovative approach.

"Non-hybrid" design is less restrictive, more productive, and 1000 times better for those of us who are "organizo-centric". That is to say, I can arrange all of my sketches in a "sketches" geometrical set, planes in a "planes" geomeetrical set, so on and so forth. I can also sub-order them. All of this without EVER having to worry about breaking logical ordering.

If being neurotic was one of your favorite things about Pro/E, you can still do that in Catia. You can do it ways that are much more fun, in fact.

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