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boolean operation

boolean operation

boolean operation

(OP)
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?

RE: boolean operation

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.

RE: boolean operation

(OP)
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?

RE: boolean operation

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

RE: boolean operation

Quote:

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.

-----------------------------------------------------------
Catia Design|Catia Design News|Catia V5 blog

RE: boolean operation

(OP)
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 !

RE: boolean operation

Quote (par1):


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

Yes, you do.

-----------------------------------------------------------
Catia Design|Catia Design News|Catia V5 blog

RE: boolean operation

(OP)
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?

RE: boolean operation

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

RE: boolean operation

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..


RE: boolean operation


correction for my previous posting

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

RE: boolean operation

(OP)
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?

RE: boolean operation

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.

RE: boolean operation

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.

RE: boolean operation

Quote:

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)

-----------------------------------------------------------
Catia Design|Catia Design News|Catia V5 blog

RE: boolean operation

Quote:

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.  

RE: boolean operation

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.. :)

RE: boolean operation

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.

RE: boolean operation

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

Quote (Stargazer81):

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.

-----------------------------------------------------------
Catia Design|Catia Design News|Catia V5 blog

RE: boolean operation

Stargazer81- I came from UG and it is very linear in its data, same as Pro/E.  I didn't like V5 at first but now that I am creating loads of data and also editing the data that is not cumbersome due to a linear requirement, my speed has increased.  

Sure there are differances but that is what makes it interesting.  Amazing how many threads end up to the hybrid/no hybrid debate.

RE: boolean operation

Quote (solid7):

You are what I like to call "tainted".

Yes! I know I am and that's why had to admit it. And I have read some of your posts in another thread so I know that you are QUITE familiar with this. I was talking about the "experts" in my company. (We doesn't have a standard to follow yet.)

I do have my opinion, but I may change this if someone convinces me that "your" way is better.

Quote (solid7):

I can arrange all of my sketches in a "sketches" geometrical set

This is very interresting.. I want to have all my sketches ordered directly under each feature. Why do you need them in an geo-set? Doesn't this mean that you have to set the geo-set as active every time you make a new sketch? And if you need to change the sketch plane later to some other surface that you have to pick in the middle of your tree? Or if you have projected/intersected someting from your solid at a certain time. How do you "find back" to the same place in the tree as when you created the sketch the first time to replace these? Don't you get update cycles?

I also have a question regarding the original subject of this thread (since we are a bit of-track):
I have a quite large and complex part whit many booleans, and suddenly when i try to assemble one more body Catia refuses to move it under the PartBody as all the others. Even if i put it at the end and if i sketch a simple circle with no links to anything above.. Are currently running R14, and when I do the same in R16 this works. Just a bug?

RE: boolean operation

Stargazer - you can move your sketch after creation.  Contextual menu - change geometric set -- pick a different partbody or geometric set.  Having sketches in common area would make it easy for another user to find what they are looking for.  If you create a pad, draft all sides, add some fillets..... it can be cumbersome to find the initial sketch.
What colour is the gear of the Partbody?  the only time I have seen this - Hybrid and Non-Hybrids in the same part, but this could be a R14 bug.

Regards,
Derek

RE: boolean operation

Quote (Stargazer81):

I want to have all my sketches ordered directly under each feature. Why do you need them in an geo-set? Doesn't this mean that you have to set the geo-set as active every time you make a new sketch?

First off, not it does not.  Derek stated correctly, that you can move them after creation, very easily.  I have  my left arrow button set as a hot key to change geometrical sets, as I do a lot of organizing at the end.  Why don't I want sketches in the PartBody, you wonder?  Because I'm a neat freak when it comes to data, and I don't like part trees that look like the great wall of China.  I prefer to have like elements grouped similarly.  It's much easier to find things that way.

Just for fun, Stargazer81 - would you like to compare one of my part trees to one of your hybrid trees?

To address something else that you said - it is just plain wrong to attach sketches to surfaces, or other features, unless you have a 100% sound reason to do so.  YOu are asking for update errors in doing such.  Wherever possible, it is much better to let elements be parametric, but independent of features.  I like to think of it this way:  Features from elements, but no elements from features.

As for the hybrid bodies issue, I fear this to be a bug.  I tried it in R14, but it worked for me, and no problem on later releases. (I have a lot of customer data that is translated from UG, and it all comes in as hybrid bodies, so I deal with this alot) Of course, you haven't mentioned what release and SP you are using.  You can search the IBM website for a PMR on this issue.

-----------------------------------------------------------
Catia Design|Catia Design News|Catia V5 blog

RE: boolean operation

Just to chime in I organize like Solid7.  Although we have hybrid bodies enabled, I never put wireframe/surface/GSD elements in my part bodies.  

Instead I goup by geometric sets like Sketches, Planes, IML / OML Surfaces, Inspection Points, etc...

I find this to be a great way of organization as long as you use descriptive names for your sketches.  


Maybe its just a preferenece thing, but I HATE having long part body history trees as well.  

RE: boolean operation

It's more than just preference, long solid body trees tend to update at a sluggish pace.

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