Hybrid Design 2

[thixoguy]

Hi All,

I know the topic of hybrid design has been discussed in other threads,some people are for it others against. I am fairly new to Catia (5 months) and I have just started playing around with hybrid design. From what I have seen so far I feel quite comfortable working in it as it is very similar to the the way UG works and thats the software I used prior to Catia. I have a few questions that I was hoping other more experienced users might address.

1.What are some of the problems you might encounter if you switch over to hybrid design? Will legacy data present any problems? Is there a way to easily identify a file created in hybrid mode?

2.How do catia users with previous UG experience prefer to work? Please provide some advantages/disadvantages or short comings with this method and some possible simple examples that might enlighten me.

3. Why did catia even bother introducing hybrid design? Did it exist in V4?

4.I would greatly appreciate any comments both for and against hybrid design. I think it is the way I would like to work in the future but before doing so I would like to gather as much information as I can so I know what I may be up against.

A big thanks to all who take the time to provide input.

thixoguy

 

[jackk]

Thixoguy,

Here's my opinions on your questions. Please note that we do not use Hybrid Design where I work, primarily because it is different from what our 200+ users are familiar with.

1. If you feel comfortable using Hybrid Design - go for it. The only problems I forsee is if someone else has to work with your parts and they are not familiar with the different tree structure. Another problem is if you decide to convert your part to non-hybrid, as I've found it is very difficult to do. Another problem is Update Cycle errors - you'll problem get many more of them if you use sloppy, Non-Hybrid organization versus structured (ordered) geometry.

2. never used UG, so I can't compare

3. As someone pointed out in another post, Hybrid Design was introduced in order to meet the requirements of a large automotive company. CATIA V4 does not have a hierarchial database like V5 and it does not have a Spec Tree to organize data, so it is impossible to answer. V4 does combine wireframe/surface/solids geometry into a single data file and everything can be used together like in V5.

4. The advantages of Hybrid Design include: better geometry organzation, and better PowerCopy capabilities. The disadvantage is that it's new and confusing to long time users.

Some things to consider before deciding which way to go:

5. Are you the only CATIA user at your company? Or will other users modify your parts in the future? Does everyone want (or are they willing) to start using it?

6. Do your customers use Hybrid Design?. Will your customers be confused if they try to modify your parts?

 

[thixoguy]

jackk,

I want to thank you for taking the time to offer your input. You have definately raised some important issues that I should consider if and when I decide to switch over to hybrid design. Your insight is much appreciated.

thixoguy

 

[slcad]

I was wondering what company is jackk talking about... Most of the "big players" our company works for (BMW, VAG) specifically demand NOT TO USE HYBRID DESIGN...

Just now I´m running into a hybrid-design matter... I have a part with a loooooong specification tree, where some bodies were accidentally inserted (and used) while Hybrid design was activated. Of course, this falls against our customer´s demands!

Now, my question: is there any quicker way to FIND all those bodies, other than browsing a 50 screen-full long specification tree to find the different-colored icons?

Any help would be greatly appreciated... Thanks in advance!

Stely

 

[itsmyjob]

Do not look in europe to find the large automotive company.

go east...

Eric N.
indocti discant et ament meminisse periti ​

 

[jackk]

Stely,

I was repeating what I had read some time ago in another forum.

I was told later that Toyota requested this capability (and Volumes) in order to convert their legacy data to CATIA V5.

I also heard that Honda does not use Hybrid Design.

(both companies must have some super education and support - you never see anyone from either company on these forums)

I recall hearing that someone had a quality check program that could identify parts containing Hybrid bodies. I think it might have been BMW (but I'm not sure).

Maybe someone else can verify this, or provide some info for you on how to write a script or macro.

...Jack

 

[slcad]

Thanks Jack,

meanwhile I found a "middleway", using "Parametrization Analysis" I located pretty quick the "guilty" ones...

Regards,
Stely

 

[jackk]

Stely,

Thanks for the tip on Parametrization Analysis - it does a nice job listing all the bodies so you can quickly see which ones are Hybrid.

Now the fun begins!

Let us know how your cleanup goes. I found it easiest to erase and start over.

 

[slcad]

Hi Jack,

I used a mixture of your solutions posted in the Apr.5-6 thread. Mostly I tried to use power-copies (thanks eklunja for the suggestion!) but there were some situations where I couldn´t use them (i.e. when I used faces of a "root" dummy-solid to create/constrain sketches). There I would do copy-paste into a non-hybrid body (including features like fillets and so on that can be copy-pasted!), than replaced the hybrid body with the non-hybrid one. Actually I use quite often the "Replace" contextual command, it works great!

Of course some the subsequent "drafts" and "fillets" needed some re-routing, but I completed my task in 2 hours, much less than finding the solution . Luckily, there were only 9 (out of 200+) "guilty" bodies to be replaced, and the 2 hours were spent mostly waiting for the workstation to do all the calculation (it´s a ca. 75M file!) than to do the work itself...

Regards,
Stely